Summary of Content for Mitsubishi M70 Machining Center System Programming Manual PDF
MELDAS is a registered trademark of Mitsubishi Electric Corporation. Other company and product names that appear in this manual are trademarks or registered trademarks of the respective companies.
Introduction
This manual is a guide for using the MITSUBISHI CNC 700/70 Series. Programming is described in this manual, so read this manual thoroughly before starting programming. Thoroughly study the «Precautions for Safety» on the following page to ensure safe use of this NC unit. Details described in this manual
CAUTION
For items described in «Restrictions» or «Usable State», the instruction manual issued by the machine tool builder takes precedence over this manual.
An effort has been made to note as many special handling methods in this user’s manual. Items not described in this manual must be interpreted as «not possible».
This manual has been written on the assumption that all option functions are added. Refer to the specifications issued by the machine tool builder before starting use.
Refer to the Instruction Manual issued by each machine tool builder for details on each machine tool. Some screens and functions may differ depending on the NC system or its version, and some
functions may not be possible. Please confirm the specifications before use.
General precautions
(1) Refer to the following documents for details on handling MITSUBISHI CNC 700/70 Series Instruction Manual …………………………… IB-1500042
Precautions for Safety Always read the specifications issued by the machine maker, this manual, related manuals and attached documents before installation, operation, programming, maintenance or inspection to ensure correct use. Understand this numerical controller, safety items and cautions before using the unit. This manual ranks the safety precautions into «DANGER», «WARNING» and «CAUTION».
When the user may be subject to imminent fatalities or major injuries if handling is mistaken. When the user may be subject to fatalities or major injuries if handling is mistaken. When the user may be subject to injuries or when physical damage may occur if handling is mistaken.
Note that even items ranked as » CAUTION«, may lead to major results depending on the situation. In any case, important information that must always be observed is described.
DANGER
Not applicable in this manual.
WARNING
Not applicable in this manual.
CAUTION
1. Items related to product and manual
For items described as «Restrictions» or «Usable State» in this manual, the instruction manual issued by the machine tool builder takes precedence over this manual.
An effort has been made to describe special handling of this machine, but items that are not described must be interpreted as «not possible».
This manual is written on the assumption that all option functions are added. Refer to the specifications issued by the machine tool builder before starting use.
Refer to the Instruction Manual issued by each machine tool builder for details on each machine tool.
Some screens and functions may differ depending on the NC system or its version, and some functions may not be possible. Please confirm the specifications before use.
(Continued on next page)
DANGER
WARNING
CAUTION
CAUTION
2. Items related to operation
Before starting actual machining, always carry out dry operation to confirm the machining program, tool compensation amount and workpiece offset amount, etc.
If the workpiece coordinate system offset amount is changed during single block stop, the new setting will be valid from the next block.
Turn the mirror image ON and OFF at the mirror image center.
Refer to the Instruction Manual issued by each machine tool builder for details on each machine tool.
If the tool compensation amount is changed during automatic operation (including during single block stop), it will be validated from the next block or blocks onwards.
3. Items related to programming
The commands with «no value after G» will be handled as «G00».
EOB», «%», and EOR are symbols used for explanation. The actual codes for ISO are «CR, LF» («LF») and «%». The programs created on the Edit screen are stored in the NC memory in a «CR, LF» format, however, the programs created with external devices such as the FLD or RS-232C may be stored in an «LF» format.
The actual codes for EIA are «EOB (End of Block)» and «EOR (End of Record)».
When creating the machining program, select the appropriate machining conditions, and make sure that the performance, capacity and limits of the machine and NC are not exceeded. The examples do not consider the machining conditions.
Do not change fixed cycle programs without the prior approval of the machine tool builder.
When programming a program of the multi-part system, carefully observe the movements caused by other part systems’ programs.
Contents
1. Control Axes………………………………………………………………………………………………………………….1 1.1 Coordinate Words and Control Axis…………………………………………………………………………….1 1.2 Coordinate Systems and Coordinate Zero Point Symbols………………………………………………2
2. Least Command Increments…………………………………………………………………………………………..3 2.1 Input Setting Units…………………………………………………………………………………………………….3 2.2 Input Command Increment Tenfold……………………………………………………………………………..5 2.3 Indexing Increment……………………………………………………………………………………………………6
3. Data Formats …………………………………………………………………………………………………………………7 3.1 Tape Codes……………………………………………………………………………………………………………..7 3.2 Program Formats ……………………………………………………………………………………………………10 3.3 Tape Memory Format………………………………………………………………………………………………13 3.4 Optional Block Skip …………………………………………………………………………………………………13
3.4.1 Optional Block Skip; /…………………………………………………………………………………………13 3.4.2 Optional Block Skip Addition ; /n………………………………………………………………………….14
3.5 Program/Sequence/Block Numbers ; O, N …………………………………………………………………16 3.6 Parity H/V ………………………………………………………………………………………………………………17 3.7 G Code Lists ………………………………………………………………………………………………………….18 3.8 Precautions Before Starting Machining………………………………………………………………………21
4. Buffer Register …………………………………………………………………………………………………………….22 4.1 Input Buffer…………………………………………………………………………………………………………….22 4.2 Pre-read Buffers……………………………………………………………………………………………………..23
5. Position Commands …………………………………………………………………………………………………….24 5.1 Position Command Methods ; G90, G91 ……………………………………………………………………24 5.2 Inch/Metric Command Change; G20, G21………………………………………………………………….26 5.3 Decimal Point Input …………………………………………………………………………………………………28
6. Interpolation Functions ………………………………………………………………………………………………..33 6.1 Positioning (Rapid Traverse); G00…………………………………………………………………………….33 6.2 Linear Interpolation; G01………………………………………………………………………………………….40 6.3 Plane Selection; G17, G18, G19……………………………………………………………………………….42 6.4 Circular Interpolation; G02, G03 ……………………………………………………………………………….44 6.5 R-specified Circular Interpolation; G02, G03 ………………………………………………………………49 6.6 Helical Interpolation ; G17 to G19, G02, G03 ……………………………………………………………..52 6.7 Thread Cutting ……………………………………………………………………………………………………….56
6.7.1 Constant Lead Thread Cutting ; G33……………………………………………………………………56 6.7.2 Inch Thread Cutting; G33……………………………………………………………………………………60
6.8 Unidirectional Positioning; G60…………………………………………………………………………………61 6.9 Cylindrical Interpolation; G07.1 …………………………………………………………………………………63 6.10 Polar Coordinate Interpolation; G12.1, G13.1/G112,G113 ………………………………………….71 6.11 Exponential Function Interpolation; G02.3, G03.3 ……………………………………………………..78 6.12 Polar Coordinate Command ; G16/G15 ……………………………………………………………………84 6.13 Spiral/Conical Interpolation; G02.0/G03.1(Type1), G02/G03(Type2) ……………………………90 6.14 3-dimensional Circular Interpolation; G02.4, G03.4 ……………………………………………………95 6.15 NURBS Interpolation……………………………………………………………………………………………100 6.16 Hypothetical Axis Interpolation; G07 ………………………………………………………………………105
7. Feed Functions ………………………………………………………………………………………………………….107 7.1 Rapid Traverse Rate ……………………………………………………………………………………………..107 7.2 Cutting Feedrate …………………………………………………………………………………………………..107 7.3 F1-digit Feed………………………………………………………………………………………………………..108 7.4 Feed Per Minute/Feed Per Revolution
(Asynchronous Feed/Synchronous Feed); G94, G95 …………………………………………………110
7.5 Inverse Time Feed; G93 ………………………………………………………………………………………..112 7.6 Feedrate Designation and Effects on Control Axes ……………………………………………………116 7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration …………………………………..120 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration ……………………122 7.9 Exact Stop Check; G09………………………………………………………………………………………….131 7.10 Exact Stop Check Mode; G61……………………………………………………………………………….134 7.11 Deceleration Check……………………………………………………………………………………………..134
7.11.1 G1 -> G0 Deceleration Check………………………………………………………………………….136 7.11.2 G1 -> G1 Deceleration Check………………………………………………………………………….137
7.12 Automatic Corner Override; G62……………………………………………………………………………138 7.13 Tapping Mode; G63 …………………………………………………………………………………………….143 7.14 Cutting Mode ; G64 ……………………………………………………………………………………………..143
8. Dwell………………………………………………………………………………………………………………………….144 8.1 Per-second Dwell ; G04 …………………………………………………………………………………………144
9. Miscellaneous Functions ……………………………………………………………………………………………146 9.1 Miscellaneous Functions (M8-digits BCD) ………………………………………………………………..146 9.2 Secondary Miscellaneous Functions (B8-digits, A8 or C8-digits) …………………………………148 9.3 Index Table Indexing……………………………………………………………………………………………..149
10. Spindle Functions…………………………………………………………………………………………………….151 10.1 Spindle Functions (S6-digits Analog) ……………………………………………………………………..151 10.2 Spindle Functions (S8-digits) ………………………………………………………………………………..151 10.3 Constant Surface Speed Control; G96, G97……………………………………………………………152
10.3.1 Constant Surface Speed Control ……………………………………………………………………..152 10.4 Spindle Clamp Speed Setting; G92 ……………………………………………………………………….153 10.5 Spindle/C Axis Control …………………………………………………………………………………………154 10.6 Multiple Spindle Control ……………………………………………………………………………………….157
10.6.1 Multiple Spindle Control II ……………………………………………………………………………….158
11. Tool Functions (T command)…………………………………………………………………………………….160 11.1 Tool Functions (T8-digit BCD)……………………………………………………………………………….160
12. Tool Compensation Functions ………………………………………………………………………………….161 12.1 Tool Compensation ……………………………………………………………………………………………..161 12.2 Tool Length Compensation/Cancel; G43, G44/G49 …………………………………………………165 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G49…………………………….168 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42………………………………………………175
12.4.1 Tool radius Compensation Operation ……………………………………………………………….176 12.4.2 Other Commands and Operations during Tool Radius Compensation…………………..185 12.4.3 G41/G42 Commands and I, J, K Designation…………………………………………………….194 12.4.4 Interrupts during Tool Radius Compensation …………………………………………………….200 12.4.5 General Precautions for Tool Radius Compensation…………………………………………..202 12.4.6 Changing of Compensation No. during Compensation Mode……………………………….203 12.4.7 Start of Tool Radius Compensation and Z Axis Cut in Operation………………………….205 12.4.8 Interference Check ………………………………………………………………………………………..207 12.4.9 Diameter Designation of Compensation Amount………………………………………………..214 12.4.10 Workpiece Coordinate Changing during Radius Compensation………………………….216
12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42…………………………………218 12.6 Tool Position Offset; G45 to G48 …………………………………………………………………………..229 12.7 Programmed Compensation Input ; G10, G11…………………………………………………………236 12.8 Inputting the Tool Life Management Data; G10, G11 ……………………………………………….241
12.8.1 Inputting the Tool Life Management Data by G10 L3 Command…………………………..241 12.8.2 Inputting the Tool Life Management Data by G10 L30 Command…………………………243 12.8.3 Precautions for Inputting the Tool Life Management Data……………………………………246
13. Program Support Functions ……………………………………………………………………………………..247 13.1 Fixed Cycles……………………………………………………………………………………………………….247
13.1.1 Standard Fixed Cycles; G80 to G89, G73, G74, G75, G76 ………………………………….247 13.1.2 Drilling Cycle with High-Speed Retract ……………………………………………………………..274 13.1.3 Initial Point and R Point Level Return; G98, G99………………………………………………..277 13.1.4 Setting of Workpiece Coordinates in Fixed Cycle Mode………………………………………278
13.2 Special Fixed Cycle; G34, G35, G36, G37.1 …………………………………………………………..279 13.3 Subprogram Control; M98, M99, M198…………………………………………………………………..284
13.3.1 Calling Subprogram with M98 and M99 Commands …………………………………………..284 13.3.2 Calling Subprogram with M198 Commands ………………………………………………………289 13.3.3 Figure Rotation; M98 I_ J_ K_ …………………………………………………………………………289
13.4 Variable Commands…………………………………………………………………………………………….292 13.5 User Macro Specifications ……………………………………………………………………………………297
13.5.1 User Macro Commands; G65, G66, G66.1, G67………………………………………………..297 13.5.2 Macro Call Command …………………………………………………………………………………….298 13.5.3 ASCII Code Macro …………………………………………………………………………………………307 13.5.4 Variables………………………………………………………………………………………………………311 13.5.5 Types of Variables …………………………………………………………………………………………313 13.5.6 Arithmetic Commands…………………………………………………………………………………….351 13.5.7 Control Commands ………………………………………………………………………………………..356 13.5.8 External Output Commands…………………………………………………………………………….359 13.5.9 Precautions…………………………………………………………………………………………………..361 13.5.10 Actual Examples of Using User Macros…………………………………………………………..363
13.6 G Command Mirror Image; G50.1, G51.1……………………………………………………………….367 13.7 Corner Chamfering/Corner Rounding I …………………………………………………………………..370
13.7.1 Corner Chamfering » ,C_ » ………………………………………………………………………………370 13.7.2 Corner Rounding » ,R_ » …………………………………………………………………………………372
13.8 Linear Angle Command ……………………………………………………………………………………….373 13.9 Geometric Command …………………………………………………………………………………………..374 13.10 Circle Cutting; G12, G13 …………………………………………………………………………………….378 13.11 Parameter Input by Program; G10, G11 ……………………………………………………………….380 13.12 Macro Interrupt; M96, M97………………………………………………………………………………….381 13.13 Tool Change Position Return; G30.1 to G30.6 ………………………………………………………389 13.14 Normal Line Control ; G40.1/G41.1/G42.1…………………………………………………………….392 13.15 High-accuracy Control ; G61.1, G08 …………………………………………………………………….403 13.16 High-speed Machining Mode ; G05, G05.1……………………………………………………………417
13.16.1 High-speed Machining Mode I,II ; G05 P1, G05 P2…………………………………………..417 13.17 High-speed High-accuracy Control ; G05, G05.1……………………………………………………420
13.17.1 High-speed High-accuracy Control I, II ……………………………………………………………420 13.17.2 SSS Control ………………………………………………………………………………………………..427
13.18 Spline; G05.1 ……………………………………………………………………………………………………432 13.19 High-accuracy Spline Interpolation ; G61.2……………………………………………………………439 13.20 Scaling ; G50/G51……………………………………………………………………………………………..441 13.21 Coordinate Rotation by Program; G68/G69 …………………………………………………………..446 13.22 Coordinate Rotation Input by Parameter; G10……………………………………………………….453 13.23 3-dimensional Coordinate Conversion ; G68/69 …………………………………………………….456 13.24 Tool Center Point Control; G43.4/G43.5 ……………………………………………………………….473 13.25 Timing-synchronization between Part Systems ……………………………………………………..495
14. Coordinates System Setting Functions ……………………………………………………………………..498 14.1 Coordinate Words and Control Axes………………………………………………………………………498 14.2 Basic Machine, Workpiece and Local Coordinate Systems……………………………………….499 14.3 Machine Zero Point and 2nd, 3rd, 4th Reference Positions……………………………………….500 14.4 Basic Machine Coordinate System Selection; G53…………………………………………………..501 14.5 Coordinate System Setting ;G92……………………………………………………………………………502 14.6 Automatic Coordinate System Setting ……………………………………………………………………503 14.7 Reference (Zero) Position Return; G28, G29…………………………………………………………..504 14.8 2nd, 3rd and 4th Reference (Zero) Position Return; G30 ………………………………………….508
14.9 Reference Position Check; G27…………………………………………………………………………….511 14.10 Workpiece Coordinate System Setting and Offset ; G54 to G59 (G54.1) …………………..512 14.11 Local Coordinate System Setting; G52 …………………………………………………………………524 14.12 Workpiece Coordinate System Preset; G92.1 ……………………………………………………….528 14.13 Coordinate System for Rotary Axis ………………………………………………………………………533
15. Measurement Support Functions………………………………………………………………………………536 15.1 Automatic Tool Length Measurement; G37 …………………………………………………………….536 15.2 Skip Function; G31………………………………………………………………………………………………540 15.3 Multi-step Skip Function; G31.n, G04 …………………………………………………………………….545 15.4 Multi-step Skip Function 2; G31 …………………………………………………………………………….547 15.5 Speed Change Skip; G31 …………………………………………………………………………………….549 15.6 Programmable Current Limitation ………………………………………………………………………….552 15.7 Stroke Check before Travel; G22/G23……………………………………………………………………553
Appendix 1. Program Error ………………………………………………………………………………………….555 Appendix 2. Order of G Function Command Priority……………………………………………………..575 INDEX …………………………………………………………………………………………………………………………… X-1
1. Control Axes 1.1 Coordinate Words And Control Axis
1
1. Control Axes 1.1 Coordinate Words and Control Axis
Function and purpose
In the standard specifications, there are 3 control axes, but, by adding an additional axis, up to 4 axes can be controlled. The designation of the processing direction responds to those axes and uses a coordinate word made up of alphabet characters that have been decided beforehand.
Program coordinates
Direction of table movement
Direction of table movement
Bed
X-Y table
+Z
+Z +Y
+X
+X +Y
Workpiece
X-Y table
Program coordinates Direction of table movement Direction of table
revolution
+Z +C
+X +X
+Y
+Y
+C
Workpiece
X-Y and revolving table
1. Control Axes 1.2 Coordinate Systems And Coordinate Zero Point Symbols
2
1.2 Coordinate Systems and Coordinate Zero Point Symbols Function and purpose
: Reference position
: Machine coordinate zero point
: Workpiece coordinate zero points (G54 — G59)
Basic machine coordinate system
Machine zero point
1st reference position Workpiece
coordinate system 3 (G56)
Workpiece coordinate system 2 (G55)
Workpiece coordinate system 1 (G54)
Workpiece coordinate system 6 (G59)
Workpiece coordinate system 5 (G58)
Workpiece coordinate system 4 (G57)
Local coordinate system (G52)
-Y
y3
-X
y2
y
y1
y5
x1
x3 x2
x
x5
2. Least Command Increments 2.1 Input Setting Units
3
2. Least Command Increments 2.1 Input Setting Units
Function and purpose
The input setting units are, as with the compensation amounts, the units of setting data used in common for all axes. The command units are the movement amounts in the program which are commanded with MDI inputs or command tape. These are expressed with mm, inch or degree () units. With the parameters, the command units are decided for each axis, and the input setting units are decided commonly for all axes.
Linear axis Parameters
Millimeter Inch Rotation axis
()
#1003 iunit = B 0.001 0.0001 0.001 = C 0.0001 0.00001 0.0001 = D 0.00001 0.000001 0.00001
Input setting unit
= E 0.000001 0.0000001 0.000001 #1015 cunit = 0 Follow #1003 iunit = 1 0.0001 0.00001 0.0001 = 10 0.001 0.0001 0.001 = 100 0.01 0.001 0.01 = 1000 0.1 0.01 0.1
Command unit
= 10000 1.0 0.1 1.0
(Note 1) Inch/metric changeover is performed in either of 2 ways: conversion from the parameter
screen (#1041 I_inch: valid only when the power is turned ON) and conversion using the G command (G20 or G21).
However, when a G command is used for the conversion, the conversion applies only to the input command increments and not to the input setting units.
Consequently, the tool offset amounts and other compensation amounts as well as the variable data should be preset to correspond to inches or millimeters.
(Note 2) The millimeter and inch systems cannot be used together. (Note 3) During circular interpolation on an axis where the input command increments are
different, the center command (I, J, K) and the radius command (R) can be designated by the input setting units. (Use a decimal point to avoid confusion.)
2. Least Command Increments 2.1 Input Setting Units
4
Detailed description
(1) Units of various data
These input setting units determine the parameter setting unit, program command unit and the external interface unit for the PLC axis and handle pulse, etc. The following rules show how the unit of each data changes when the input setting unit is changed. This table applies to the NC axis and PLC axis.
Input setting unit Data Unit
system Setting value 1m (B) 0.1m (C) 10nm (D) 1nm (E)
20000 (mm/min) 20000 20000 20000 20000Milli- metre Setting range 1 to 999999 1 to 999999 1 to 999999 1 to 999999
2000 (inch/min) 2000 2000 2000 2000
Speed data Example: rapid Inch
Setting range 1 to 999999 1 to 999999 1 to 999999 1 to 999999 123.123 (mm) 123.123 123.1230 123.12300 123.123000Milli-
metre Setting range 99999.999 99999.9999 99999.99999 99999.999999 12.1234 (inch) 12.1234 12.12340 12.123400 12.1234000
Position data Example: SoftLimit+ Inch
Setting range 9999.9999 9999.99999 9999.999999 9999.9999999 1 (m) 2 20 200 2000Milli-
metre Setting range 9999 9999 9999 9999 0.001 (inch) 2 20 200 2000
Interpolation unit data Inch
Setting range 9999 9999 9999 9999 (2) Program command
The program command unit follows the above table. If the data has a decimal point, the number of digits in the integer section will remain and the number of digits in the decimal point section will increase as the input setting unit becomes smaller. When setting data with no decimal point, and which is a position command, the data will be affected by the input setting increment and input command increment. For the feed rate, as the input setting unit becomes smaller, the number of digits in the integer section will remain the same, but the number of digits in the decimal point section will increase.
2. Least Command Increments 2.2 Input Command Increment Tenfold
5
2.2 Input Command Increment Tenfold Function and purpose
The program’s command increment can be multiplied by an arbitrary scale with the parameter designation. This function is valid when a decimal point is not used for the command increment. The scale is set with the parameters.
Detailed description
(1) When running a machining program already created with a 10m input command increment
with a CNC unit for which the command increment is set to 1m and this function’s parameter value is set to «10», machining similar to before this function is possible.
(2) When running a machining program already created with a 1m input command increment
with a CNC unit for which the command increment is set to 0.1m and this function’s parameter value is set to «10», machining similar to before this function is possible.
(3) This function cannot be used for the dwell function G04_X_(P_);. (4) This function cannot be used for the compensation amount of the tool compensation input. (5) This function can be used when decimal point type I is valid, but cannot be used when decimal
point type II is valid.
«UNIT*10» parameter Program example (Machining program:
programmed with 1=10m) (CNC unit is 1=1m system) 10 1
X Y X Y N1 G90 G00 X0 Y0; 0 0 0 0 N2 G91 X-10000 Y-15000; -100.000 -150.000 -10.000 -15.000 N3 G01 X-10000 Y-5000 F500; -200.000 -200.000 -20.000 -20.000 N4 G03 X-10000 Y-10000 J-10000; -300.000 -300.000 -30.000 -30.000 N5 X10000 Y-10000 R5000; -200.000 -400.000 -20.000 -40.000 N6 G01 X20.000 Y.20.000 -180.000 -380.000 0.000 -20.000
N1
N2
N3
N4
N5
R
-400
-300
-200
-100
W
-100 -200 -300
N6
UNIT*10 ON
N1
N2
N3
N4
N5
R
-40
-30
-20
-10
W
-10 -20 -30
N6
UNIT*10 OFF
2. Least Command Increments 2.3 Indexing Increment
6
2.3 Indexing Increment
Function and purpose
This function limits the command value for the rotary axis. This can be used for indexing the rotary table, etc. It is possible to cause a program error with a program command other than an indexing increment (parameter setting value).
Detailed description
When the indexing increment (parameter) for limiting the command value is set, the rotary axis can be positioned with that indexing increment. If a program other than the indexing increment setting value is commanded, a program error (P20) will occur. The indexing position will not be checked when the parameter is set to 0. (Example) When the indexing increment setting value is 2 degrees, only command with the
2-degree increment are possible.
G90 G01 C102. 000 ; Moves to the 102 degree angle. G90 G01 C101. 000 : Program error G90 G01 C102 ; Moves to the 102 degree angle. (Decimal point type II)
The following axis specification parameter is used.
# Item Contents Setting range (unit)
2106 Index unit Indexing increment
Set the indexing increment to which the rotary axis can be positioned.
0 to 360 ( )
Precautions
When the indexing increment is set, degree increment positioning takes place. The indexing position is checked with the rotary axis, and is not checked with other axes. When the indexing increment is set to 2 degrees, the rotary axis is set to the B axis, and the B
axis is moved with JOG to the 1.234 position, an indexing error will occur if «G90B5.» or «G91B5.» is commanded.
3. Data Formats 3.1 Tape Codes
7
3. Data Formats 3.1 Tape Codes
Function and purpose
The tape command codes used for this controller are combinations of alphabet letters (A, B, C, … Z), numbers (0, 1, 2 … 9) and signs (+, -, / …). These alphabet letters, numbers and signs are referred to as characters. Each character is represented by a combination of 8 holes which may, or may not, be present. These combinations make up what is called codes. This controller uses, the ISO code (R-840).
(Note 1) If a code not given in the tape code table in Fig. 1 is assigned during operation, program
error (P32) will result. (Note 2) For the sake of convenience, a semicolon » ; » has been used in the CNC display to
indicate the end of a block (EOB/IF) which separates one block from another. Do not use the semicolon key, however, in actual programming but use the keys in the following table instead.
CAUTION EOB», «%», and EOR are symbols used for explanation. The actual codes for ISO are «CR, LF» («LF») and «%». The programs created on the Edit screen are stored in the NC memory in a «CR, LF» format, however, the programs created with external devices such as the FLD or RS-232C may be stored in an «LF» format. The actual codes for EIA are «EOB (End of Block)» and «EOR (End of Record)».
Detailed description
EOB/EOR keys and displays Code used
Key used ISO Screen display
End of block LF or NL ; End of record % %
(1) Significant data section (label skip function) All data up to the first EOB ( ; ), after the power has been turned on or after operation has been reset, are ignored during automatic operation based on tape, memory loading operation or during a search operation. In other words, the significant data section of a tape extends from the character or number code after the initial EOB ( ; ) code after resetting to the point where the reset command is issued.
3. Data Formats 3.1 Tape Codes
8
(2) Control out, control in
When the ISO code is used, all data between control out «(» and control in «)» or «;» are ignored, although these data appear on the setting and display unit. Consequently, the command tape name, No. and other such data not directly related to control can be inserted in this section. This information (except (B) in the tape codes) will also be loaded, however, during tape loading. The system is set to the «control in» mode when the power is witched on.
L C S L F RG0 0 X — 8 5 0 0 0 Y — 6 4 0 0 0 ( CUT T ERPRE T URN ) F
Operator information print-out example
Information in this section is ignored and nothing is executed.
Example of ISO code
(3) EOR (%) code
Generally, the end-or-record code is punched at both ends of the tape. It has the following functions: (a) Rewind stop when rewinding tape (with tape handler) (b) Rewind start during tape search (with tape handler) (c) Completion of loading during tape loading into memory
(4) Tape preparation for tape operation (with tape handler)
Initial block Last block2m
10cm %
2m
10cm %
(EOR) (EOR)(EOB) (EOB) (EOB)(EOB)
; ;;;
If a tape handler is not used, there is no need for the 2-meter dummy at both ends of the tape and for the head EOR (%) code.
3. Data Formats 3.1 Tape Codes
9
8 7 6 5 4 3 2 1 Channel No.
1 2
3 4
5 6
7 8
9 0
A B
C D
E F
G H
I J
K L
M N
O P
Q R
S T
U V
W X
Y Z
+ — .
, / %
LF(Line Feed) or NL ( (Control Out)
) (Control In) :
# * = [ ] SP(Space) CR(Carriage Return) BS(Back Space)
HT(Horizontal Tab) &
! $ ‘ (Apostrophe)
; <
> ?
@ «
DEL(Delete) NULL
DEL(Delete)
Under the ISO code, IF or NL is EOB and % is EOR. Under the ISO code, CR is meaningless, and EOB will not occur.
A
B
ISO code (R-840) Feed holes
Code A are stored on tape but an error results (except when they are used in the comment section) during operation. The B codes are non-working codes and are always ignored. Parity V check is not executed.
Table of tape codes
3. Data Formats 3.2 Program Formats
10
3.2 Program Formats
Function and purpose
The prescribed arrangement used when assigning control information to the controller is known as the program format, and the format used with this controller is called the «word address format».
Detailed description
(1) Word and address
A word is a collection of characters arranged in a specific sequence. This entity is used as the unit for processing data and for causing the machine to execute specific operations. Each word used for this controller consists of an alphabet letter and a number of several digits (sometimes with a «-» sign placed at the head of the number.).
*
Alphabet (address)
Word
Numerals
Word configuration
The alphabet letter at the head of the word is the address. It defines the meaning of the numerical information which follows it. For details of the types of words and the number of significant digits of words used for this controller, refer to the «format details».
(2) Blocks
A block is a collection of words. It includes the information which is required for the machine to execute specific operations. One block unit constitutes a complete command. The end of each block is marked with an EOB (end-of-block) code.
(Example 1)
G0X — 1000 ; G1X — 2000F500 ; 2 blocks
(Example 2)
(G0X — 1000 ; ) G1X — 2000F500 ;
Since the semicolon in the parentheses will not result in an EOB, it is 1 block.
(3) Programs
A program is a collection of several blocks.
3. Data Formats 3.2 Program Formats
11
Metric command Inch command Rotary axis
(Metric command) Rotary axis
(Inch command) Program No. 08 Sequence No. N6 Preparatory function G3/G21
0.001() mm/ 0.001 inch X+53 Y+53 Z+53 +53 X+44 Y+44 Z+44 +44 X+53 Y+53 Z+53 +53 X+53 Y+53 Z+53 +53
0.0001() mm/ 0.0001 inch X+54 Y+54 Z+54 +54 X+45 Y+45 Z+45 +45 X+54 Y+54 Z+54 +54 X+54 Y+54 Z+54 +54
0.00001() mm/ 0.00001 inch X+55 Y+55 Z+55 +55 X+46 Y+46 Z+46 +46 X+55 Y+55 Z+55 +55 X+55 Y+55 Z+55 +55
Movement axis
0.000001() mm/ 0.000001 inch X+56 Y+56 Z+56 +56 X+47 Y+47 Z+47 +47 X+56 Y+56 Z+56 +56 X+56 Y+56 Z+56 +56
0.001() mm/ 0.001 inch I+53 J+53 K+53 I+44 J+44 K+44 I+53 J+53 K+53 I+53 J+53 K+53
(Note 5) 0.0001() mm/ 0.0001 inch I+54 J+54 K+54 I+45 J+45 K+45 I+54 J+54 K+54 I+54 J+54 K+54
(Note 5) 0.00001() mm/ 0.00001 inch I+55 J+55 K+55 I+46 J+46 K+46 I+55 J+55 K+55 I+55 J+55 K+55
(Note 5)
Arc and cutter radius
0.000001() mm/ 0.000001 inch I+56 J+56 K+56 I+47 J+47 K+47 I+56 J+56 K+56 I+56 J+56 K+56
(Note 5) Dwell 0.001(rev)/(s) X53/P8
0.001() mm/ 0.001 inch F63 F54 F63 F54 (Note 6)
0.0001 () mm/ 0.0001 inch F64 F55 F64 F55 (Note 6)
0.00001 () mm/ 0.00001 inch F65 F56 F65 F56 (Note 6)
Feed function (Feed per minute)
0.000001 () mm/ 0.000001 inch F66 F57 F66 F57 (Note 6)
0.0001() mm/ 0.0001 inch F33 F34 F33 F34 (Note 6)
0.00001 () mm/ 0.00001 inch F34 F35 F34 F35 (Note 6)
0.000001 () mm/ 0.000001 inch F35 F36 F35 F36 (Note 6)
Feed function (Feed per revolution)
0.0000001 () mm/ 0.0000001 inch F36 F37 F36 F37 (Note 6)
Tool compensation H3 D3 Miscellaneous function (M) M8 Spindle function (S) S8 Tool function (T) T8 2nd miscellaneous function A8/B8/C8 Subprogram P8 H5 L4
0.001() mm/ 0.001 inch R+53 Q53 P8 L4 R+44 Q44 P8 L4 R+53 Q53 P8 L4 R+53 Q53 P8 L4
0.0001() mm/ 0.0001 inch R+54 Q54 P8 L4 R+45 Q45 P8 L4 R+54 Q54 P8 L4 R+54 Q54 P8 L4
0.00001() mm/ 0.00001 inch R+55 Q55 P8 L4 R+46 Q46 P8 L4 R+55 Q55 P8 L4 R+55 Q55 P8 L4
Fixed cycle
0.000001() mm/ 0.000001 inch R+56 Q56 P8 L4 R+47 Q47 P8 L4 R+56 Q56 P8 L4 R+56 Q56 P8 L4
(Note 1) indicates the additional axis address, such as A, B or C.
(Note 2) The number of digits check for a word is carried out with the maximum number of digits of that address.
(Note 3) Numerals can be used without the leading zeros.
3. Data Formats 3.2 Program Formats
12
(Note 4) The description of the brief summary is explained below: Example 1 : 08 :8-digit program No. Example 2 : G21 :Dimension G is 2 digits to the left of the decimal point, and 1 digit to the right. Example 3 : X+53 :Dimension X uses + or — sign and represents 5 digits to the left of the decimal
point and 3 digits to the right. For example, the case for when the X axis is positioned (G00) to the 45.123 mm position in the absolute value (G90) mode is as follows:
G00 X45.123 ;
3 digits below the decimal point
5 digits above the decimal point, so it’s +00045, but the leading zeros and the mark (+) have been omitted. G0 is possible, too.
(Note 5) If an arc is commanded using a rotary axis and linear axis while inch commands are being used, the
degrees will be converted into 0.1 inches for interpolation.
(Note 6) While inch commands are being used, the rotary axis speed will be in increments of 10 degrees. Example: With the F1. (per-minute-feed) command, this will become the 10 degrees/minute command.
(Note 7) The decimal places below the decimal point are ignored when a command, such as an S command, with an invalid decimal point has been assigned with a decimal point.
(Note This format is the same for the value input from the memory, MDI or setting and display unit.
(Note 9) Command the program No. in an independent block. Command the program No. in the head block of the program.
3. Data Formats 3.3 Tape Memory Format
13
3.3 Tape Memory Format
Function and purpose
(1) Storage tape and significant sections
The others are about from the current tape position to the EOB. Accordingly, under normal conditions, operate the tape memory after resetting. The significant codes listed in «Table of tape codes» in «3.1 Tape Codes» in the above significant section are actually stored into the memory. All other codes are ignored and are not stored. The data between control out «(» and control in «)» are stored into the memory.
3.4 Optional Block Skip 3.4.1 Optional Block Skip; /
Function and purpose
This function selectively ignores specific blocks in a machining program which starts with the «/» (slash) code.
Detailed description
(1) Provided that the optional block skip switch is ON, blocks starting with the «/» code are ignored.
They are executed if the switch is OFF. Parity check is valid regardless of whether the optional block skip switch is ON or OFF. When, for instance, all blocks are to be executed for one workpiece but specific block are not to be executed for another workpiece, the same command tape can be used to machine different parts by inserting the «/» code at the head of those specific blocks.
Precautions for using optional block skip
(1) Put the «/» code for optional block skip at the beginning of a block. If it is placed inside the block,
it is assumed as a user macro, a division instruction.
Example : N20 G1 X25./Y25. ; ….NG (User macro, a division instruction; a program error results.)
/N20 G1 X25. Y25. ;…..OK (2) Parity checks (H and V) are conducted regardless of the optional block skip switch position. (3) The optional block skip is processed immediately before the pre-read buffer. Consequently, it is not possible to skip up to the block which has been read into the pre-read
buffer. (4) This function is valid even during a sequence number search. (5) All blocks with the «/» code are also input and output during tape storing and tape output,
regardless of the position of the optional block skip switch.
3. Data Formats 3.4 Optional Block Skip
14
3.4.2 Optional Block Skip Addition ; /n Function and purpose
Whether the block with «/n (n:1 to 9)» (slash) is executed during automatic operation and searching is selected. By using the machining program with «/n» code, different parts can be machined by the same program.
Detailed description
The block with «/n» (slash) code is skipped when the «/n» is programmed to the head of the block and the optional block skip signal is turned ON. For the block with the «/n» code inside the block (not the head of block), the program is operated according to the value of the parameter «#1226 aux10/bit1» setting. When the optional block skip signal is OFF, the block with «/n» is executed.
Example of program
(1) When the 2 parts like the figure below are machined, the following program is used. When the
optional block skip 5 signal is ON, the part 1 is created. When the optional block skip 5 signal is OFF, the part 2 is created. N1 G54; N2 G90G81X50. Z-20. R3. F100; /5 N3 X30.; N4 X10.; N5 G80; M02;
Part 1 the optional block skip 5 signal ON
Part 2 the optional block skip 5 signal OFF
N4 N2 N2 N3 N4
3. Data Formats 3.4 Optional Block Skip
15
(2) When two or more «/n» codes are commanded to the head of the same block, the block is
ignored if either of the optional block skip signal corresponding to the command is ON.
N01 G90 Z3. M03 S1000; /1/2 N02 G00 X50.; /1/2 N03 G01 Z-20. F100; /1/2 N04 G00 Z3.; /1 /3 N05 G00 X30.; /1 /3 N06 G01 Z-20. F100; /1 /3 N07 G00 Z3.; /2/3 N08 G00 X10.; /2/3 N09 G01 Z-20. F100; /2/3 N10 G00 Z3.; N11 G28 X0 M05; N12 M02;
(a) Optional block skip 1 signal ON (Optional block skip 2, 3 signals OFF)
N01 -> N08 -> N09 -> N10 -> N11 -> N12 (b) Optional block skip 2 signal ON
(Optional block skip 1, 3 signals OFF) N01 -> N05 -> N06 -> N07 -> N11 -> N12 (c) Optional block skip 3 signal ON
(Optional block skip 1, 2 signals OFF) N01 -> N02 -> N03 -> N04 -> N11 -> N12
(3) When the parameter «#1226 aux10/bit1» is «1», when two or more «/n» are commanded inside
the same block, the commands following «/n» in the block are ignored if either of the optional block skip signal corresponding to the command is ON.
N01 G91 G28 X0.Y0.Z0.;
N02 G01 F1000;
N03 X1. /1 Y1. /2 Z1.;
N04 M30;
(a) When the optional block skip 1 signal is ON and the optional block skip 2 signal is OFF, «Y1. Z1.» is ignored
(b) When the optional block skip 1 signal is
OFF and the optional block skip 2 signal is ON, «Z1.» is ignored.
3. Data Formats 3.5 Program/Sequence/Block Numbers ; O, N
16
3.5 Program/Sequence/Block Numbers ; O, N
Function and purpose
These numbers are used for monitoring the execution of the machining programs and for calling both machining programs and specific stages in machining programs. (1) Program numbers are classified by workpiece correspondence or by subprogram units, and
they are designated by the address «0» followed by a number with up to 8 digits. (2) Sequence numbers are attached where appropriate to command blocks which configure
machining programs, and they are designated by the address «N» followed by a number with up to 6 digits.
(3) Block numbers are automatically provided internally. They are preset to zero every time a program number or sequence number is read, and they are counted up one at a time unless program numbers or sequence numbers are commanded in blocks which are subsequently read.
Consequently, all the blocks of the machining programs given in the table below can be determined without further consideration by combinations of program numbers, sequence numbers and block numbers.
Monitor display Machining program Program No. Sequence No. Block No.
O12345678 (DEMO, PROG) ; 12345678 0 0 G92 X0 Y0 ; 12345678 0 1 G90 G51 X-150. P0.75 ; 12345678 0 2 N100 G00 X-50. Y-25. ; 12345678 100 0 N110 G01 X250. F300 ; 12345678 110 0 Y-225. ; 12345678 110 1 X-50. ; 12345678 110 2 Y-25.; 12345678 110 3 N120 G51 Y-125. P0.5 ; 12345678 120 0 N130 G00 X-100. Y-75. ; 12345678 130 0 N140 G01 X-200. ; 12345678 140 0 Y-175. ; 12345678 140 1 X-100. ; 12345678 140 2 Y-75. ; 12345678 140 3 N150 G00 G50 X0 Y0 ; 12345678 150 0 N160 M02 ; 12345678 160 0 %
3. Data Formats 3.6 Parity H/V
17
3.6 Parity H/V
Function and purpose
Parity check provides a mean of checking whether the tape has been correctly perforated or not. This involves checking for perforated code errors or, in other words, for perforation errors. There are two types of parity check: Parity H and Parity V.
(1) Parity H
Parity H checks the number of holes configuring a character and it is done during tape operation, tape input and sequence number search. A parity H error is caused in the following cases. (a) ISO code
When a code with an odd number of holes in a significant data section has been detected. (b) EIA code
When a code with an even number of holes in a significant data section has been detected.
Parity H error example
This character causes a parity H error. When a parity H error occurs, the tape stops following the alarm code.
(2) Parity V
A parity V check is done during tape operation, tape input and sequence number search when the I/O PARA #9n15 (n is the unit No.1 to 5) parity V check function is set to «1». It is not done during memory operation. A parity V error occurs in the following case: when the number of codes from the first significant code to the EOB (;) in the significant data section in the vertical direction of the tape is an odd number, that is, when the number of characters in one block is odd. When a parity V error is detected, the tape stops at the code following the EOB (;).
(Note 1) Among the tape codes, there are codes which are counted as characters for parity
and codes which are not counted as such. For details, refer to the «Table of tape codes» in «3.1 Tape Codes».
(Note 2) Any space codes which may appear within the section from the initial EOB code to the address code or «/» code are counted for parity V check.
3. Data Formats 3.7 G Code Lists
18
3.7 G Code Lists
Function and purpose
G code Group Function Section 00 01 Positioning 6.1 01 01 Linear interpolation 6.2
02 01 Circular interpolation CW (clockwise) R-specified circular interpolation CW Helical interpolation CW Spiral/Conical interpolation CW (type 2)
6.4 6.5 6.6 6.13
03 01 Circular interpolation CCW (counterclockwise) R-specified circular interpolation CCW Helical interpolation CCW Spiral/Conical interpolation CCW (type 2)
6.4 6.5 6.6 6.13
02.1 01 Spiral/Conical interpolation CW (type1) 6.13 03.1 01 Spiral/Conical interpolation CCW (type1) 6.13 02.3 01 Exponential function interpolation positive rotation 6.11 03.3 01 Exponential function interpolation negative rotation 6.11 02.4 01 3-dimensional circular interpolation 6.14 03.4 01 3-dimensional circular interpolation 6.14 04 00 Dwell 8.1 05 00 High-speed machining mode
High-speed high-accuracy control II 13.16 13.17
05.1 00 High-speed high-accuracy control I Spline
13.17 13.18
06.2 01 NURBS interpolation 6.15 07 00 Hypothetical axis interpolation 6.16 07.1 107 21 Cylindrical interpolation 6.9
08 00 High-accuracy control 13.15 09 00 Exact stop check 7.9 10 00 Program data input (parameter /compensation data/parameter
coordinate rotation data) 12.7
13.11 13.22
11 00 Program data input cancel 12.7 13.11
12 00 Circular cut CW (clockwise) 13.10 13 00 Circular cut CCW (counterclockwise) 13.10 12.1 112 21 Polar coordinate interpolation ON 6.10
* 13.1 113 21 Polar coordinate interpolation cancel 6.10
14 * 15 18 Polar coordinate command OFF 6.12
16 18 Polar coordinate command ON 6.12 17 02 Plane selection X-Y 6.3 18 02 Plane selection Z-X 6.3 19 02 Plane selection Y-Z 6.3 20 06 Inch command 5.2 21 06 Metric command 5.2
3. Data Formats 3.7 G Code Lists
19
G code Group Function Section
22 04 Stroke check before travel ON 15.7 23 04 Stroke check before travel cancel 15.7 24 25 26 27 00 Reference position check 14.9 28 00 Reference position return 14.7 29 00 Start position return 14.7 30 00 2nd to 4th reference position return 14.8 30.1 00 Tool change position return 1 13.13 30.2 00 Tool change position return 2 13.13 30.3 00 Tool change position return 3 13.13 30.4 00 Tool change position return 4 13.13 30.5 00 Tool change position return 5 13.13 30.6 00 Tool change position return 6 13.13 31 00 Skip
Multi-step skip function 2 15.2 15.4
31.1 00 Multi-step skip function 1-1 15.3 31.2 00 Multi-step skip function 1-2 15.3 31.3 00 Multi-step skip function 1-3 15.3 32 33 01 Thread cutting 6.7 34 00 Special fixed cycle (bolt hole circle) 13.2 35 00 Special fixed cycle (line at angle) 13.2 36 00 Special fixed cycle (arc) 13.2 37 00 Automatic tool length measurement 15.1 37.1 00 Special fixed cycle (grid) 13.2 38 00 Tool radius compensation vector designation 12.4 39 00 Tool radius compensation corner arc 12.4
* 40 07 Tool radius compensation cancel 3-dimentional tool radius compensation cancel
12.4 12.5
41 07 Tool radius compensation left 3-dimentional tool radius compensation left
12.4 12.5
42 07 Tool radius compensation right 3-dimentional tool radius compensation right
12.4 12.5
* 40.1 15 Normal line control cancel 13.14 41.1 15 Normal line control left ON 13.14 42.1 15 Normal line control right ON 13.14 43 08 Tool length compensation (+) 12.2 44 08 Tool length compensation (-) 12.2 43.1 08 Tool length compensation along the tool axis 12.3 43.4 08 Tool center point control type 1 13.24 43.5 08 Tool center point control type 2 13.24 45 00 Tool position offset (extension) 12.6 46 00 Tool position offset (reduction) 12.6 47 00 Tool position offset (doubled) 12.6 48 00 Tool position offset (halved) 12.6
* 49 08 Tool length compensation cancel Tool center point control cancel
12.2 13.24
* 50 11 Scaling cancel 13.20 51 11 Scaling ON 13.20
3. Data Formats 3.7 G Code Lists
20
G code Group Function Section * 50.1 19 G command mirror image cancel 13.6
51.1 19 G command mirror image ON 13.6 52 00 Local coordinate system setting 14.11 53 00 Basic machine coordinate system selection 14.4
* 54 12 Workpiece coordinate system 1 selection 14.10 55 12 Workpiece coordinate system 2 selection 14.10 56 12 Workpiece coordinate system 3 selection 14.10 57 12 Workpiece coordinate system 4 selection 14.10 58 12 Workpiece coordinate system 5 selection 14.10 59 12 Workpiece coordinate system 6 selection 14.10 54.1 12 Workpiece coordinate system selection 48 / 96 sets extended 14.10 60 00 Unidirectional positioning 6.8 61 13 Exact stop check mode 7.10 61.1 13 High-accuracy control 1 ON 13.15 61.2 13 High-accuracy spline interpolation 13.19 62 13 Automatic corner override 7.12 63 13 Tapping mode 7.13 63.1 13 Synchronous tapping mode (normal tapping) 63.2 13 Synchronous tapping mode (reverse tapping)
* 64 13 Cutting mode 7.14 65 00 User macro call 13.5.1 66 14 User macro modal call A 13.5.1 66.1 14 User macro modal call B 13.5.1
* 67 14 User macro modal call cancel 13.5.1 68 16 Programmable coordinate rotation mode ON/3-dimensional
coordinate conversion mode ON 13.21 13.23
* 69 16 Programmable coordinate rotation mode OFF/3-dimensional coordinate conversion mode OFF
13.21 13.23
70 09 User fixed cycle 71 09 User fixed cycle 72 09 User fixed cycle 73 09 Fixed cycle (step) 13.1.1 74 09 Fixed cycle (reverse tap) 13.1.1 75 09 Fixed cycle (circle cutting cycle) 13.1.1 76 09 Fixed cycle (fine boring) 13.1.1 77 09 User fixed cycle 78 09 User fixed cycle 79 09 User fixed cycle
* 80 09 Fixed cycle cancel 13.1.1 81 09 Fixed cycle (drill/spot drill) 13.1.1 82 09 Fixed cycle (drill/counter boring) 13.1.1 83 09 Fixed cycle (deep drilling) 13.1.1 84 09 Fixed cycle (tapping) 13.1.1 85 09 Fixed cycle (boring) 13.1.1 86 09 Fixed cycle (boring) 13.1.1 87 09 Fixed cycle (back boring) 13.1.1 88 09 Fixed cycle (boring) 13.1.1 89 09 Fixed cycle (boring) 13.1.1
90 03 Absolute value command 5.1 91 03 Incremental command value 5.1
3. Data Formats 3.8 Precautions Before Starting Machining
21
G code Group Function Section
92 00 Coordinate system setting / Spindle clamp speed setting 14.5 92.1 00 Workpiece coordinate system pre-setting 14.12 93 05 Inverse time feed 7.5
94 05 Feed per minute (Asynchronous feed) 7.4 95 05 Feed per revolution (Synchronous feed) 7.4 96 17 Constant surface speed control ON 10.3 97 17 Constant surface speed control OFF 10.3 * 98 10 Fixed cycle Initial level return 13.1.2
99 10 Fixed cycle R point level return 13.1.2 100 to 255
00 User macro (G code call) Max. 10 13.5.2
(Note 1) Codes marked with * are codes that must be or are selected in the initial state. The codes marked with are codes that should be or are selected in the initial state by
the parameters. (Note 2) If two or more G codes from the same code are commanded, the latter G code will be
valid. (Note 3) This G code list is a list of conventional G codes. Depending on the machine, movements
that differ from the conventional G commands may be included when called by the G code macro. Refer to the Instruction Manual issued by the tool builder.
(Note 4) Whether the modal is initialized or not depends on each reset input. (1) «Reset 1»
The modal is initialized when the reset initial parameter «#1151 rstinit» turns ON. (2) «Reset 2» and «Reset & rewind»
The modal is initialized when the signal is input. (3) Resetting when emergency stop is canceled
Follows «Reset 1». (4) When modal is automatically reset at the start of individual functions such as
reference position return. Follows «Reset & rewind».
CAUTION The commands with «no value after G» will be handled as «G00».
3.8 Precautions Before Starting Machining Precautions before starting machining
CAUTION When creating the machining program, select the appropriate machining conditions so that the machine, NC performance, capacity and limits are not exceeded. The examples do not allow for the machining conditions.
Before starting actual machining, always carry out dry operation to confirm the machining program, tool compensation amount and workpiece offset amount, etc.
4. Buffer Register 4.1 Input Buffer
22
4. Buffer Register 4.1 Input Buffer
Function and purpose
When the pre-read buffer is empty during a tape operation or RS232C operation, the contents of the input buffer are immediately transferred to the pre-read buffers and, provided that the data stored in the input buffer do not exceed 250 x 4 characters, the following data (Max. 250 characters) are read and loaded into the input buffer. This buffer is designed to eliminate the operational delay originating in the readout time of the tape reader and to smooth out the block joints. The pre-reading effects are lost, however, when the block execution time is shorter than the tape readout time of the following block.
(Buffer size : 250 x 5 characters)
Tape Input buffer
Memory
Keyboard
MDI data
Mode switching
Analysis processing
Max. 5 execution blocks
Buffer 4
Arithmetic processing
Note : Data equivalent to 1 block are stored in 1 pre-read buffer.
Buffer 3
Buffer 2
Buffer 1
Pre-read buffer 5
The input buffer has a memory capacity of 250 x 5 characters (including the EOB code).
(1) The contents of the input buffer register are updated in 250-character units. (2) Only the significant codes in the significant data section are read into the input buffer. (3) When codes (including «(» and «)») are sandwiched in the control in or control out mode and the
optional block skip function is ON, the data extending from the «/» (slash) code up to the EOB code are read into the input buffer.
(4) The input buffer contents are cleared with resetting. (Note 1) The input buffer size (250 characters) differs according to the model.
4. Buffer Register 4.2 Pre-read Buffers
23
4.2 Pre-read Buffers
Function and purpose
During automatic processing, the contents of 1 block are normally pre-read so that program analysis processing is conducted smoothly. However, during tool radius compensation, a maximum of 5 blocks are pre-read for the intersection point calculation including interference check. The specifications of the data in 1 block are as follows:
(1) The data of 1 block are stored in this buffer. (2) Only the significant codes in the significant data section are read into the pre-read buffer. (3) When codes are sandwiched in the control in and control out, and the optional block skip
function is ON, the data extending from the «/» (slash) code up to the EOB code are not read into the pre-read buffer.
(4) The pre-read buffer contents are cleared with resetting. (5) When the single block function is ON during continuous operation, the pre-read buffer stores
the following block data and then stops operation.
Other precautions
(1) Depending on whether the program is executed continuously or by single blocks, the timing of
the valid/invalid for the external control signals for the block skip and others will differ. (2) If the external control signal such as optional block skip is turned ON/OFF with the M
command, the external control operation will not be effective on the program pre-read with the buffer register.
(3) According to the M command that operates the external controls, it prohibits pre-reading, and the recalculation is as follows:
The M command that commands the external controls is distinguished at the PLC, and the «recalculation request» for PLC -> NC interface table is turned ON.
(When the «recalculation request» is ON, the program that has been pre-read is reprocessed.)
5. Position Commands 5.1 Position Command Methods; G90, G91
24
5. Position Commands 5.1 Position Command Methods ; G90, G91
Function and purpose
By using the G90 and G91 commands, it is possible to execute the next coordinate commands using absolute values or incremental values. The R-designated circle radius and the center of the circle determined by I, J, K are always incremental value commands.
Command format
G9D X__ Y__ Z__ __; G90 :Absolute command G91 :Incremental command :Additional axis
Detailed description
(1) Regardless of the current position, in the absolute
value mode, it is possible to move to the position of the workpiece coordinate system that was designated in the program.
N 1 G90 G00 X0 Y0 ;
In the incremental value mode, the current position is the start point (0), and the movement is made only the value determined by the program, and is expressed as an incremental value.
N 2 G90 G01 X200. Y50. F100;
N 2 G91 G01 X200. Y50. F100;
Using the command from the 0 point in the workpiece coordinate system, it becomes the same coordinate command value in either the absolute value mode or the incremental value mode.
(2) For the next block, the last G90/G91 command that was given becomes the modal.
(G90) N 3 X100. Y100.;
The axis moves to the workpiece coordinate system X = 100mm and Y = 100mm position.
(G91) N 3 X-100. Y50.;
The X axis moves to -100.mm and the Y axis to +50.0mm as an incremental value, and as a result X moves to 100.mm and Y to 100.mm.
Tool
300.200.
200.
100. N1
100. N2
W X
Y
300.200.
200.
100.
N3
W X
Y
100.
5. Position Commands 5.1 Position Command Methods; G90, G91
25
(3) Since multiple commands can be issued in the same block, it is possible to command specific
addresses as either absolute values or incremental values.
N 4 G90 X300. G91 Y100.;
The X axis is treated in the absolute value mode, and with G90 is moved to the workpiece coordinate system 300.mm position. The Y axis is moved +100.mm with G91. As a result, Y moves to the 200.mm position. In terms of the next block, G91 remains as the modal and becomes the incremental value mode.
(4) When the power is turned ON, it is possible to select whether you want absolute value
commands or incremental value commands with the #1073 I_Absm parameter. (5) Even when commanding with the manual data input (MDI), it will be treated as a modal from
that block.
300.200. 100.
N4
W X
Y
100.
200.
5. Position Commands 5.2 Inch/Metric Command Change; G20, G21
26
5.2 Inch/Metric Command Change; G20, G21
Function and purpose
These G commands are used to change between the inch and millimeter (metric) systems.
Command format
G20/G21; G20 : Inch command G21 : Metric command
Detailed description
The G20 and G21 commands merely select the command units. They do not select the Input units. G20 and G21 selection is meaningful only for linear axes and it is meaningless for rotation axes.
Output unit, command unit and setting unit
The counter or parameter setting and display unit is determined by parameter «#1041 I_inch». For the movement/speed command, the followings will be resulted: The movement/speed command will be displayed as metric units when «#1041 I_inch» is ON during the G21 command mode. The internal unit metric data of the movement/speed command will be converted into an inch unit and displayed when «#1041 I_inch» is OFF during the G20 command mode. The command unit for when the power is turned ON and reset is decided by combining the parameters «#1041 I_inch», «#1151 rstint» and «#1210 RstGmd/bit5». NC axis
Initial inch OFF (metric internal unit)
#1041 I_inch=0
Initial inch ON (inch internal unit)
#1041 I_inch=1 Item
G21 G20 G21 G20 Movement/ speed command Metric Inch Metric Inch
Counter display Metric Metric Inch Inch Speed display Metric Metric Inch Inch User parameter setting/display Metric Metric Inch Inch
Workpiece/ tool offset setting/display
Metric Metric Inch Inch
Handle feed command Metric Metric Inch Inch
PLC axis
Item #1042 pcinch=0 (metric)
#1042 pcinch=1 (inch)
Movement/ speed command Metric Inch
Counter display Metric Inch User parameter setting/display Metric Inch
5. Position Commands 5.2 Inch/Metric Command Change; G20, G21
27
Precautions
(1) The parameter and tool data will be input/output with the «#1041 I_inch» setting unit.
If «#1041 I_inch» is not found in the parameter input data, the unit will follow the unit currently set to NC.
(2) The unit of read/write used in PLC window is fixed to metric unit regardless of a parameter and G20/G21 command modal.
(3) A program error (P33) will occur if G20/G21 command is issued in the same block as following G code. Command in a separate block. G05 (High-speed machining mode) G7.1 (Cylindrical Interpolation) G12.1 (Polar coordinate interpolation)
5. Position Commands 5.3 Decimal Point Input
28
5.3 Decimal Point Input
Function and purpose
This function enables the decimal point command to be input. It assigns the decimal point in millimeter or inch units for the machining program input information that defines the tool paths, distances and speeds. The parameter «#1078 Decpt2» selects whether type I (minimum input command unit) or type II (zero point) is to apply for the least significant digit of data without a decimal point.
Detailed description
(1) The decimal point command is valid for the distances, angles, times, speeds and scaling rate,
in machining programs. (Note, only after G51) (2) In decimal point input type 1 and type 2, the values of the data commands without the decimal
points are shown in the table below. Command Command unit Type 1 Type 2
cunit = 10000 1000 (m, 10-4 inch, 10-3 ) 1 (mm, inch, ) cunit = 1000 100 1 cunit = 100 10 1
X1 ;
cunit = 10 1 1 (3) The valid addresses for the decimal points are X, Y, Z, U, V, W, A, B, C, I, J, K, E, F, P, Q, and
R. However, P is valid only during scaling. For details, refer to the list. (4) In decimal point command, the valid range of command value is as shown below. (Input
command unit cunit = 10)
Movement command (linear)
Movement command (rotary) Feedrate Dwell
Input unit [mm]
-99999.999 to 99999.999
0. 001 to 10000000.000
Input unit [inch]
-9999.9999 to 9999.9999
-99999.999 to 99999.999 0. 0001 to
1000000.0000
0 to 99999.999
(5) The decimal point command is valid even for commands defining the variable data used in
subprograms. (6) While the smallest decimal point command is validated, the smallest unit for a command
without a decimal point designation is the smallest command input unit set in the specifications (1m, 10m, etc.) or mm can be selected. This selection can be made with parameter «#1078 Decpt2».
(7) Decimal point commands for decimal point invalid addresses are processed as integer data
only and everything below the decimal point is ignored. Addresses which are invalid for the decimal point are D, H, L, M, N, O, S and T. All variable commands, however, are treated as data with decimal points.
(8) «Input command increment tenfold» is applied in the decimal point type I mode, but not in the
decimal point type II mode.
5. Position Commands 5.3 Decimal Point Input
29
Example of program
(1) Example of program for decimal point valid address
Decimal point command 1 Specification division
Program example When 1 = 1m When 1 = 10m
Decimal point command 2
1 = 1mm G0X123.45 (decimal points are all mm points)
X123.450mm X123.450mm X123.450mm
G0X12345 X12.345mm (last digit is 1m unit)
X123.450mm X12345.000mm
#111 = 123, #112 = 5.55 X#111 Y#112
X123.000mm, Y5.550mm
X123.000mm, Y5.550mm
X123.000mm, Y5.550mm
#113 = #111+#112 (addition) #113 = 128.550 #113 = 128.550 #113 = 128.550
#114 = #111-#112 (subtraction) #114 = 117.450 #114 = 117.450 #114 = 117.450
#115 = #111#112 (multiplication) #115 = 682.650 #115 = 682.650 #115 = 682.650
#116 = #111/#112 #117 = #112/#111 (division)
#116 = 22.162 #117 = 0.045
#116 = 22.162 #117 = 0.045
#116 = 22.162 #117 = 0.045
Decimal point input I/II and decimal point command valid/invalid
If a command does not use a decimal point at an address where a decimal point command is valid in the table on the following page, it is handled differently between decimal point input I and II modes as explained below. A command using a decimal point is handled the same way in either the decimal point input I or II mode.
(1) Decimal point input I
The least significant digit place of command data corresponds to the command unit. (Example) Command «X1» in the 1m system is equivalent to command «X0.001».
(2) Decimal point input II
The least significant digit place of command data corresponds to the decimal point. (Example) Command «X1» in the 1m system is equivalent to command «X1.».
(Note) When a four rules operator is contained, the data will be handled as that with a decimal
point.
(Example) When the min. input command unit is 1m : G0 x 123 + 0 ; … X axis 123mm command. It will not be 123m.
5. Position Commands 5.3 Decimal Point Input
30
Addresses used and validity/invalidity of decimal point commands are shown below.
Address Decimal point command Application Remarks
A Valid Coordinate position data Invalid Revolving table Invalid Miscellaneous function code Valid Angle data Invalid Data settings, axis numbers (G10)
B Valid Coordinate position data Invalid Revolving table Invalid Miscellaneous function code
C Valid Coordinate position data Invalid Revolving table Invalid Miscellaneous function code
Valid Corner chamfering amount ,c D Invalid Compensation numbers (tool position, tool radius)
Valid Automatic tool length measurement: deceleration distance d
Invalid Data setting: byte type data Invalid Subprogram storing device number ,D
E Valid Inch thread: number of ridges, precision thread: lead
F Valid Feedrate, automatic tool length measurement speed Valid Thread lead Valid Number of Z axis pitch in synchronous tap
G Valid Preparatory function code H Invalid Tool length compensation number
Invalid Sequence numbers in subprograms Invalid Program parameter input: bit type data Invalid Basic spindle selection
I Valid Arc center coordinates, center of figure rotation Valid Tool radius compensation vector components Valid Hole pitch in the special fixed cycle Valid Circle radius of cut circle (increase amount) Valid G0/G1 imposition width, drilling cycle G0 imposition width ,I Valid Stroke check before travel: lower limit coordinates
J Valid Arc center coordinates, center of figure rotation Valid Tool radius compensation vector components Valid Special fixed cycle’s hole pitch or angle Valid G0/G1 imposition width, drilling cycle G1 imposition width Valid Stroke check before travel: lower limit coordinates
5. Position Commands 5.3 Decimal Point Input
31
Address Decimal point command Application Remarks
K Valid Arc center coordinates, center of figure rotation Valid Tool radius compensation vector components Invalid Number of holes of the special fixed cycle Invalid Number of drilling cycle repetitions Valid Stroke check before travel: lower limit coordinates
L Invalid Number of fixed cycle and subprogram repetitions Invalid Program tool compensation input/workpiece offset input:
type selection L2, L20, L12, L10, L13, L11
Invalid Program parameter input: data setting selection L70 Invalid Program parameter input: 2-word type data 4
bytes Invalid Tool life data
M Invalid Miscellaneous function codes N Invalid Sequence numbers
Invalid Program parameter input: data numbers O Invalid Program numbers P Invalid/Valid Dwell time Param
eter Invalid Subprogram program call: program No. Invalid/Valid Dwell at tap cycle hole base Param
eter Invalid Number of holes of the special fixed cycle Invalid Amount of helical pitch Invalid Offset number (G10) Invalid Constant surface speed control axis number Invalid Program parameter input: broad classification number Invalid Multi-step skip function 2 signal command Invalid Subprogram return destination sequence No. Invalid 2nd, 3rd, 4th reference position return number Valid Scaling magnification Invalid High-speed mode type Invalid Extended workpiece coordinate system No. Invalid Tool life data group No.
Q Valid Cut amount of deep hole drill cycle Valid Shift amount of back boring Valid Shift amount of fine boring Invalid Minimum spindle clamp speed Valid Starting shift angle for screw cutting Invalid Tool life data management method
5. Position Commands 5.3 Decimal Point Input
32
Address Decimal point command Application Remarks
R Valid R-point in the fixed cycle Valid R-specified arc radius Valid Corner R arc radius ,R Valid Offset amount (G10) Invalid Synchronous tap/asynchronous tap changeover Valid Automatic tool length measurement: deceleration
distance r
Valid Rotation angle S Invalid Spindle function codes
Invalid Maximum spindle clamp speed Invalid Constant surface speed control: surface speed Invalid Program parameter input: word type data 2
bytes T Invalid Tool function codes U Valid Coordinate position data V Valid Coordinate position data W Valid Coordinate position data X Valid Coordinate position data
Valid Dwell time Y Valid Coordinate position data Z Valid Coordinate position data
(Note 1) All decimal points are valid for the user macro arguments.
6. Interpolation Functions 6.1 Positioning (Rapid Traverse)
33
6. Interpolation Functions 6.1 Positioning (Rapid Traverse); G00
Function and purpose
This command is accompanied by coordinate words. It positions the tool along a linear or non-linear path from the present point as the start point to the end point which is specified by the coordinate words.
Command format
G00 X__ Y__ Z__ __ ; ( represents additional axis) X, Y, Z, : Represent coordinates, and could be either absolute values or
incremental values, depending on the setting of G90/G91.
Detailed description
(1) Once this command has been issued, the G00 mode is retained until it is changed by another
G function or until the G01, G02, G03 or G33 command in the 01 group is issued. If the next command is G00, all that is required is simply that the coordinate words be specified.
(2) In the G00 mode, the tool is always accelerated at the start point of the block and decelerated
at the end point. Having no more command pulse in the current block and the following error status of the acceleration/deceleration paths are confirmed before advancing to the next block. The in-position width is set with the parameters.
(3) Any G command (G72 to G89) in the 09 group is cancelled (G80) by the G00 command. (4) The tool path can be selected from linear or non-linear.
The positioning time is the same for the linear and non-linear paths. (a) Linear path……… : This is the same as linear interpolation (G01), and the speed is limited
by the rapid traverse rate of each axis. (b) Non-linear path .. : The tool is positioned at the rapid traverse rate independently for each
axis.
CAUTION The commands with «no value after G» will be handled as «G00».
6. Interpolation Functions 6.1 Positioning (Rapid Traverse)
34
Example of program
Unit : mm
Tool
Z
End point (-120,+200,+300)
Start point (+150,-100,+150)
X Y
+300
+150
+200+150
-120 -100
G91 G00 X-270000 Y300000 Z150000 ; (For input setting unit: 0.001mm)
(Note 1) When parameter «#1086 G0Intp» is set to «0», the path along which the tool is positioned is the shortest path connecting the start and end points. The positioning speed is automatically calculated so that the shortest distribution time is obtained in order that the commanded speeds for each axis do not exceed the rapid traverse rate.
When for instance, the Y axis and Z axis rapid traverse rates are both 9600mm/min, the tool will follow the path in the figure below if the following is programmed:
G91 G00 X-300000 Y200000 ; (With an input setting unit of 0.001mm)
End point Actual Y axis rate : 6400mm/min
Actual X axis rate : 9600mm/min
Start point (Unit : mm)
fx
fy
Y
X
300
20 0
6. Interpolation Functions 6.1 Positioning (Rapid Traverse)
35
(Note 2) When parameter «#1086 G0Intp» is set to 1, the tool will move along the path from the start point to
the end point at the rapid traverse rate of each axis. When, for instance, the Y axis and Z axis rapid traverse rates are both 9600mm/min, the tool will
follow the path in the figure below if the following is programmed: G91 G00 X-300000 Y200000 ; (With an input setting unit of 0.001mm)
End point Actual Y axis rate : 9600mm/min
Actual X axis rate : 9600mm/min
Start point (Unit : mm)
fx
fy
Y
X
300
20 0
(Note 3) The rapid traverse rate for each axis with the G00 command differs according to the individual machine and so reference should be made to the machine specifications.
6. Interpolation Functions 6.1 Positioning (Rapid Traverse)
36
(Note 4) Rapid traverse (G00) deceleration check There are two methods for the deceleration check at rapid traverse; commanded deceleration
method and in-position check method. Select a method with the parameter «#1193 inpos».
When «inpos» = «1» Upon completion of the rapid traverse (G00), the next block will be executed after confirming that
the remaining distances for each axis are below the fixed amounts. (Refer to following drawing.) The confirmation of the remaining distance should be done with the imposition width, LR . L R is the
setting value for the servo parameter «#2224 SV 024». The purpose of checking the rapid feedrate is to minimize the time it takes for positioning. The
bigger the setting value for the servo parameter «#2224 SV024», the longer the reduced time is, but the remaining distance of the previous block at the starting time of the next block also becomes larger, and this could become an obstacle in the actual processing work. The check for the remaining distance is done at set intervals. Accordingly, it may not be possible to get the actual amount of time reduction for positioning with the setting value SV 024.
When «inpos» = «0»
Upon completion of the rapid traverse (G00), the next block will be executed after the deceleration check time (Td) has elapsed. The deceleration check time (Td) is as follows, depending on the acceleration/deceleration type.
(1) Linear acceleration/linear deceleration…………………………………. Td = Ts +
Ts
Td
Previous block Next block
Ts : Acceleration/deceleration time constant
Td : Deceleration check time Td = Ts + (0 ~ 14ms)
(2) Exponential acceleration/linear deceleration…………………………. Td = 2 Ts +
2 Ts
Td Ts
Previous block Next block
Ts : Acceleration/deceleration time constant
Td : Deceleration check time Td = 2 Ts + (0 ~ 14ms)
6. Interpolation Functions 6.1 Positioning (Rapid Traverse)
37
(3) Exponential acceleration/exponential deceleration ………………… Td = 2 Ts +
Ts
Td
Previous block Next block
Ts : Acceleration/deceleration time constant
Td : Deceleration check time Td = 2 Ts + (0 ~ 14ms)
Where Ts is the acceleration time constant, = 0 to 14ms The time required for the deceleration check during rapid traverse is the longest among the rapid
traverse deceleration check times of each axis determined by the rapid traverse acceleration/deceleration time constants and by the rapid traverse acceleration/deceleration mode of the axes commanded simultaneously.
6. Interpolation Functions 6.1 Positioning (Rapid Traverse)
38
Programmable in-position width command for positioning
This command commands the in-position width for the positioning command from the machining program.
G00 X__ Y__ Z__ , I__ ;
In-position width
Positioning coordinate value of each axis
Operation during in-position check
Execution of the next block starts after confirming that the position error amount of the positioning (rapid traverse: G00) command block and the block that carries out deceleration check with the linear interpolation (G01) command is less than the in-position width issued in this command. The in-position width in this command is valid only in the command block, so the deceleration check method set in base specification parameter «#1193 inpos» is used for blocks that do not have the in-position width command. When there are several movement axes, the system confirms that the position error amount of each movement axis in each part system is less than the in-position width issued in this command before executing the next block. The differences of when the in-position check is validated with the parameter (base specification parameter «#1193 inpos» set to 1; refer to next page for in-position width) and when validated with this command are shown in the following drawing.
Differences between in-position check with this command and in-position check with parameter
In-position check with «,I» address command In-position check with parameter After starting deceleration of the command system, the position error amount and commanded in-position width are compared.
After starting deceleration of the command system, the servo system’s position error amount and the parameter setting value (in-position width) are compared.
Servo Command
In-position width (Error amount of command end point and machine position)
Start of in-position check with «,I» address command
Block being executed
Ts
Td
In-position width (Servo system position error amount)
Start of in-position check with parameter
Servo Command
Block being executed
Ts
Td
Ts : Acceleration/deceleration time constant Td : Deceleration check time Td = Ts + (0 to 14ms)
6. Interpolation Functions 6.1 Positioning (Rapid Traverse)
39
In-position width setting
When the servo parameter «#2224 SV024» setting value is smaller than the setting value of the G0 in-position width «#2077 G0inps» and the G1 in-position width «#2078 G1inps», the in-position check is carried out with the G0 in-position width and the G1 in-position width. In-position check using the «G0inps» value Command to motor
Outline of motor movement
G0 in-position
SV024
A stop is judged here. In-position check using the «G1inps» value Command to motor
Outline of motor movement
G1 in-position
SV024
A stop is judged here.
When the SV024 value is larger, the in-position check is completed when the error amount is smaller than the SV024 setting value. The in-position check method depends on the method set in the deceleration check parameter.
(Note 1) When the in-position width (programmable in-position check width) is set in the machining program, either the in-position width set with the parameter (SV024, G0inps, G1inps) or that set in the program, whichever larger, is applied when performing an in-position check.
(Note 2) When the SV024 setting value is larger than the G0 in-position width/G1 in-position width, the in-position check is carried out with the SV024 value.
(Note 3) When the error detect is ON, the in-position check is forcibly carried out.
6. Interpolation Functions 6.2 Linear Interpolation
40
6.2 Linear Interpolation; G01
Function and purpose
This command is accompanied by coordinate words and a feedrate command. It makes the tool move (interpolate) linearly from its present position to the end point specified by the coordinate words at the speed specified by address F. In this case, the feedrate specified by address F always acts as a linear speed in the tool nose center advance direction.
Command format
G01 X__ Y__ Z__ __ F__ ,I__ ; ( represents additional axis) X, Y, Z, :Represents the coordinate value. An absolute position or
incremental position is indicated based on the state of G90/G91 at that time.
F :Feedrate (mm/min or /min) I :In-position width. This is valid only in the commanded block. A
block that does not contain this address will follow the parameter «#1193 inpos» settings.
Detailed description
(1) Once this command is issued, the mode is maintained until another G function (G00, G02, G03,
G33) in the 01 group which changes the G01 mode is issued. Therefore, if the next command is also G01 and if the feedrate is the same, all that is required to be done is to specify the coordinate words. If no F command is given in the first G01 command block, program error (P62) results.
(2) The feedrate for a rotary axis is commanded by /min (decimal point position unit). (F300 = 300/min)
(3) The G functions (G70 — G89) in the 09 group are cancelled (G80) by the G01 command.
6. Interpolation Functions 6.2 Linear Interpolation
41
Example of program
(Example 1) Cutting in the sequence of P1 P2 P3 P4 P1 at 300 mm/min feedrate P0 P1 is for tool positioning
Unit: mm Input setting unit: 0.001mmP4
P1
P0
P3 P2
20
30
20 20
30
Y
X
G90 G00 X20000 Y20000 ; P0 P1 G01 X20000 Y30000 F300 P1 P2 X30000 ; P2 P3 X-20000 Y-30000 ; P3 P4 X-30000 ; P4 P1
Programmable in-position width command for linear interpolation
This command commands the in-position width for the linear interpolation command from the machining program. The commanded in-position width is valid in the linear interpolation command only when carrying out deceleration check. When the error detect switch is ON. When G09 (exact stop check) is commanded in the same block. When G61 (exact stop check mode) is selected.
G01 X__ Y__ Z__ F__ , I__ ; In-position width
Feedrate Linear interpolation coordinate value of each axis
(Note 1) Refer to section «6.1 Positioning (rapid traverse); G00» for details on the in-position check operation.
6. Interpolation Functions 6.3 Plane Selection
42
6.3 Plane Selection; G17, G18, G19
Function and purpose
The plane to which the movement of the tool during the circle interpolation (including helical cutting) and tool radius compensation command belongs is selected. By registering the basic three axes and the corresponding parallel axis as parameters, a plane can be selected by two axes that are not the parallel axis. If the rotary axis is registered as a parallel axis, a plane that contains the rotary axis can be selected.
The plane selection is as follows: Plane that executes circular interpolation (including helical cutting) Plane that executes tool radius compensation Plane that executes fixed cycle positioning.
Command format
G17 ; G18 ; G19 ;
(ZX plane selection) (YZ plane selection) (XY plane selection)
X, Y and Z indicate each coordinate axis or the parallel axis.
Parameter entry
Table 1 Example of plane selection parameter entry #1026 to 1028
base_I,J,K #1029 to 1039
aux_I,J,K
I X U
J Y
K Z V
As shown in the above example, the basic axis and its parallel axis can be registered. The basic axis can be an axis other than X, Y and Z. Axes that are not registered are irrelevant to the plane selection.
6. Interpolation Functions 6.3 Plane Selection
43
Plane selection system
In Table 1, I is the horizontal axis for the G17 plane or the vertical axis for the G18 plane J is the vertical axis for the G17 plane or the horizontal axis for the G19 plane K is the horizontal axis for the G18 plane or the vertical axis for the G19 plane In other words, G17 ….. IJ plane G18 ….. KI plane G19 ….. JK plane (1) The axis address commanded in the same block as the plane selection (G17, G18, G19)
determines which basic axis or parallel axis is used for the plane selection. For the parameter registration example in Table 1.
G17X__Y__ ; XY plane G18X__V__ ; VX plane G18U__V__ ; VU plane G19Y__Z__ ; YZ plane G19Y__V__ ; YV plane
(2) The plane will not changeover at a block where a plane selection G code (G17, G18, G19) is
not commanded. G17X__Y__ ; XY plane
Y__Z__ ; XY plane (plane does not change)
(3) If the axis address is omitted in the block where the plane selection G code (G17, G18, G19) is commanded, it will be viewed as though the basic three axes address has been omitted. For the parameter registration example in Table 1.
G17 ; XY plane G17U__ ; UY plane G18U__ ; ZU plane G18V__ ; VX plane G19Y__ ; YZ plane G19V__ ; YV plane
(4) The axis command that does not exist in the plane determined by the plane selection G code
(G17, G18, G19) is irrelevant to the plane selection. For the parameter registration example in Table 1.
G17U__Z__ ; (5) If the above is commanded, the UY plane will be selected, and Z will move regardless of the
plane. If the basic axis and parallel axis are commanded in duplicate in the same block as the plane selection G code (G17, G18, G19), the plane will be determined in the priority order of basic axis and parallel axis. For the parameter registration example in Table 1.
G17U__Y__W__-; If the above is commanded, the UY plane will be selected, and W will move regardless of the plane. (Note 1) The plane set with parameter «#1025 I_plane» will be selected when the power is turned
ON or reset.
6. Interpolation Functions 6.4 Circular Interpolation; G02, G03
44
6.4 Circular Interpolation; G02, G03
Function and purpose
These commands serve to move the tool along an arc.
Command format
G02 (G03) X__ Y__ I__ J__ K__ F__;
G02 : Clockwise (CW) G03 : Counterclockwise (CCW) X, Y : End point I, J : Arc center F : Feedrate
For the arc command, the arc end point coordinates are assigned with addresses X, Y (or Z, or parallel axis X, Y, Z), and the arc center coordinate value is assigned with addresses I, J (or K). Either an absolute value or incremental value can be used for the arc end point coordinate value command, but the arc center coordinate value must always be commanded with an incremental value from the start point. The arc center coordinate value is commanded with an input setting unit. Caution is required for the arc command of an axis for which the input command value differs. Command with a decimal point to avoid confusion.
6. Interpolation Functions 6.4 Circular Interpolation; G02, G03
45
Detailed description
(1) G02 (or G03) is retained until another G command (G00, G01 or G33) in the 01 group that
changes its mode is issued. The arc rotation direction is distinguished by G02 and G03. G02 Clockwise (CW) G03 Counterclockwise (CCW)
Y
X
G02
G03
G02
G03
G02
G03
Y
X
Z
Z X
Z
Y G3
G3 G3
G2 G2
G2
G17(X-Y)plane G18(Z-X)plane G19(Y-Z)plane
(2) An arc which extends for more than one quadrant can be executed with a single block
command. (3) The following information is needed for circular interpolation.
(a) Plane selection ………………. : Is there an arc parallel to one of the XY, ZX or YZ planes? (b) Rotation direction …………… : Clockwise (G02) or counterclockwise (G03)? (c) Arc end point coordinates… : Given by addresses X, Y, Z (d) Arc center coordinates ……. : Given by addresses I, J, K (incremental commands) (e) Feed rate ………………………. : Given by address F
6. Interpolation Functions 6.4 Circular Interpolation; G02, G03
46
Example of program
(Example 1)
Y axis
Feedrate F = 500mm/min
Circle center J = 50mm
Start point/end point X axis
+Y
+X
G02 J50000 F500 ; Circle command
(Example 2)
Y axis
Feedrate F = 500mm/min
Start point
X axis
+Y
+X
Arc center J = 50mm
End point X50 Y50mm
G91 G02 X50000 Y50000 J50000 F500 ; 3/4 command
6. Interpolation Functions 6.4 Circular Interpolation; G02, G03
47
Plane selection
The planes in which the arc exists are the following three planes (refer to the detailed drawings), and are selected with the following method. XY plane G17; Command with a (plane selection G code) ZX plane G18; Command with a (plane selection G code) YZ plane G19; Command with a (plane selection G code)
Change into linear interpolation command
Program error (P33) will occur when the center and radius are not designated at circular command. When the parameter «#11029 Arc to G1 no Cent (Change command from arc to linear when no arc center designation)» is set, the linear interpolation can be applied to terminal coordinates value for only the block. However, a modal is the circular modal. This function is not applied to a circular command by a geometric function. (Example) The parameter «#11029 Arc to G1 no Cent (Change command from arc to linear when no arc center designation)» = «1»
N1
N3
20 0
G90 X0 Y0 ; N1 G02 X20. I10. F500 ; N2 G00 X0 N3 G02 X20. F500 ; M02 ;
(a) (b)
(a) The circular interpolation (G02) is executed because there is a center command. (b) The linear interpolation (G01) is executed because there is no center and radius command.
6. Interpolation Functions 6.4 Circular Interpolation; G02, G03
48
Precautions for circular interpolation
(1) The terms «clockwise» (G02) and «counterclockwise» (G03) used for arc operations are
defined as a case where in a right-hand coordinate system, the negative direction is viewed from the position direction of the coordinate axis which is at right angles to the plane in question.
(2) When all the end point coordinates are omitted or when the end point is the same position as the start point, a 360 arc (full circle) is commanded when the center is commanded using I, J and K.
(3) The following occurs when the start and end point radius do not match in an arc command : (a) Program error (P70) results at the arc start point when error R is greater than parameter
«#1084 RadErr».
Start point
Alarm stop
Start point radius End point radius
End point
#1084 RadErr parameter value 0.100 Start point radius = 5.000
End point radius = 4.899 Error R = 0.101
Center
(G91) G02X9.899I 5. ;
R
(b) Spiral interpolation in the direction of the commanded end point results when error R is
less than the parameter value.
Start point Start point radius End point radius
End point
#1084 RadErr parameter value 0.100 Start point radius = 5.000
End point radius = 4.900 Error R = 0.100
Spiral interpolation
Center
(G91) G02X9.9I 5. ;
R
The parameter setting range is from 0.001mm to 1.000mm.
6. Interpolation Functions 6.5 R-specified Circular Interpolation; G02, G03
49
6.5 R-specified Circular Interpolation; G02, G03
Function and purpose
Along with the conventional circular interpolation commands based on the arc center coordinate (I, J, K) designation, these commands can also be issued by directly designating the arc radius R.
Command format
G02 (G03) X__ Y__ R__ F__ ;
X : X axis end point coordinate Y : Y axis end point coordinate R : Arc radius F : Feedrate
The arc radius is commanded with an input setting unit. Caution is required for the arc command of an axis for which the input command value differs. Command with a decimal point to avoid confusion.
Detailed description
The arc center is on the bisector line which is perpendicular to the line connecting the start and end points of the arc. The point, where the arc with the specified radius whose start point is the center intersects the perpendicular bisector line, serves as the center coordinates of the arc command. If the R sign of the commanded program is plus, the arc is smaller than a semisphere; if it is minus, the arc is larger than a semisphere.
Center point
Arc path when R sign is minus
L r
Arc path when R sign is plus
End point
Center point 01
Start point
02 Center point
The following condition must be met with an R-specified arc interpolation command:
L/(2xr) 1 An error will occur when L/2 — r > (parameter : #1084 RadErr) Where L is the line from the start point to end point. When the R specification and I, J, K specification are contained in the same block, the R specification has priority in processing. When the R specification and I, J, K specification are contained in the same block, the R specification has priority in processing. The plane selection is the same as for the I, J, K-specified arc command.
6. Interpolation Functions 6.5 R-specified Circular Interpolation; G02, G03
50
Example of program
(Example 1)
G02 Xx1 Yy1 Rr1 Ff1 ; XY plane R-specified arc (Example 2)
G03 Zz1 Xx1 Rr1 Ff1 ; ZX plane R-specified arc (Example 3)
G02 Xx1 Yy1 Ii1 Jj1 Rr1 Ff1 ; XY plane R-specified arc (When the R specification and I, J, (K) specification are contained in the same block, the R specification has priority in processing.)
(Example 4)
G17 G02 Ii1 Jj1 Rr1 Ff1 ; XY plane This is an R-specified arc, but as this is a circle command, it is already completed.
6. Interpolation Functions 6.5 R-specified Circular Interpolation; G02, G03
51
Circular center coordinate compensation
When «the error margin between the segment connecting the start and end points» and «the commanded radius 2» is less than the setting value because the required semicircle is not obtained by calculation error in R specification circular interpolation, «the midpoint of segment connecting the start and end points» is compensated as the circular center. Set the setting value to the parameter «#11028 Tolerance Arc Cent (Tolerable correction value of arc center error)». (Ex.) «#11028 Tolerance Arc Cent» = «0.000 (mm)»
Setting value Tolerance value Setting value< 0 0(Center error will not be interpolated) Setting value= 0 2minimum setting increment
Setting value> 0 Setting value
0 10
N1, N3
N
G90 X0 Y0 ;
N1 G02 X10. R5.000;
N2 G0 X0;
N3 G02 X10. R5.001;
N4 G0 X0;
N5 G02 X10. R5.002;
N6 G0 X0;
M02 ;
(a)
(b)
(a) Compensate the center coordinate: Same as N1 path (b) Do not compensate the center coordinate: Inside path a little than N1 Calculation error margin compensation allowance value: 0.002 mm Segment connecting the start and end paints: 10.000 N3: Radius 2 = 10.002 «Error 0.002 -> Compensate» N5: Radius 2 = 10.004 «Error 0.004 -> Do not compensate» Therefore, this example is shown in the above figure.
6. Interpolation Functions 6.6 Helical Interpolation ; G17 to G19, G02, G03
52
6.6 Helical Interpolation ; G17 to G19, G02, G03
Function and purpose
While circular interpolating with G02/G03 within the plane selected with the plane selection G code (G17, G18, G19), the 3rd axis can be linearly interpolated. Normally, the helical interpolation speed is designated with the tangent speed F’ including the 3rd axis interpolation element as shown in the lower drawing of Fig. 1. However, when designating the arc plane element speed, the tangent speed F on the arc plane is commanded as shown in the upper drawing of Fig. 1. The NC automatically calculates the helical interpolation tangent speed F’ so that the tangent speed on the arc plane is F.
Y
Z
X
F
F
Y
X
Start point
Start point
End point
End point
Fig. 1 Designation of helical interpolation speed
Command format
G17 G02 (G03) Xx1 Yy1 Zz1 Ii1 Jj1 Pp1 Ff1 ; Helical interpolation command (Specify arc center) G17 G02 (G03) Xx2 Yy2 Zz2 Rr2 Ff2 ; Helical interpolation command (Specify radius (R)) G17(G18, G19) : Plane selection (G17: XY plane, G18: ZX plane, G19: YZ plane) G02(G03) : Arc rotation direction Xx1 Yy1 Xx2 Yy2 : Arc end point coordinate Zz1 Zz2 : Linear axis end point coordinate Ii1 Jj1 : Arc center coordinate Pp1 : Pitch No. Ff1 Ff2 : Feedrate Rr2 : Arc radius
The arc center coordinate and arc radius are commanded with an input setting input. Caution is required for the helical interpolation command of an axis for which the input command value differs. Command with a decimal point to avoid confusion. Absolute or incremental values can be assigned for the arc end point coordinates and the end point coordinates of the linear axis, but incremental values must be assigned for the arc center coordinates.
6. Interpolation Functions 6.6 Helical Interpolation ; G17 to G19, G02, G03
53
The arc plane element speed designation and normal speed designation can be selected with the parameter.
#1235 set07/bit0 Meaning 1 Arc plane element speed designation is selected. 0 Normal speed designation is selected.
Normal speed designation
Z axis
P1 time
First time
End point
Y axis
X axis
Start point
Y
X
e
s Z1
l
Second time
(1) This command should be issued with a linear axis (multiple axes can be commanded) that does not contain a circular axis in the circular interpolation command combined.
(2) For feedrate F, command the X, Y Z axis composite element directions speed. (3) Pitch l is obtained with the following expression.
l= Z1 (2 P1 + ) / 2
= E — s = tan-1 ye xe — tan-1 ys
xs (0 < 2)
Where xs, ys are the start point coordinates from the arc center xe, ye are the end point coordinates from the arc center
(4) If pitch No. is 0, address P can be omitted.
(Note) The pitch No. P command range is 0 to 9999. The pitch No. designation (P command) cannot be made with the R-specified arc.
(5) Plane selection
The helical interpolation arc plane selection is determined with the plane selection mode and axis address as for the circular interpolation. For the helical interpolation command, the plane where circular interpolation is executed is commanded with the plane selection G code (G17, G18, G19), and the 2 circular interpolation axes and linear interpolation axis (axis that intersects with circular plane) 3 axis addresses are commanded.
XY plane circular, Z axis linear Command the X, Y and Z axis addresses in the G02 (G03) and G17 (plane selection G code) mode.
ZX plane circular, Y axis linear Command the X, Y and Z axis addresses in the G02 (G03) and G18 (plane selection G code) mode.
YZ plane circular, X axis linear Command the X, Y and Z axis addresses in the G02 (G03) and G19 (plane selection G code) mode.
6. Interpolation Functions 6.6 Helical Interpolation ; G17 to G19, G02, G03
54
The plane for an additional axis can be selected as with circular interpolation.
UY plane circular, Z axis linear
Command the U, Y and Z axis addresses in the G02 (G03) and G19 (plane selection G code) mode.
In addition to the basic command methods above, the command methods following the program example can be used. Refer to the section «6.3 plane selection» for the arc planes selected with these command methods.
Example of program
(Example 1)
Z axis
Y axis
X axis
z1
G17 ; XY plane G03 Xx1 Yy1 Zz1 Ii1 Jj1 P0 Ff1 ; XY plane arc, Z axis linear
(Note) If pitch No. is 0, address P can be omitted.
Z axis
Y axis
X axis
z1 r1
(Example 2) G17 ; XY plane G02 Xx1 Yy1 Zz1 Rr1 Ff1 ; XY plane arc, Z axis linear
(Example 3)
Z axis
Y axis
U axis z1
G17 G03 Uu1 Yy1 Zz1 Ii1 Jj1 P2 Ff1 ; UY plane arc, Z axis linear
6. Interpolation Functions 6.6 Helical Interpolation ; G17 to G19, G02, G03
55
(Example 4)
U axis X axis
Z axis
u1
z1
x1
G18 G03 Xx1 Uu1 Zz1 Ii1 Kk1 Ff1 ; ZX plane arc, U axis linear (Note) If the same system is used, the standard axis will perform circular interpolation
and the additional axis will perform linear interpolation.
(Example 5) G18 G02 Xx1 Uu1 Yy1 Zz1 Ii1 Jj1 Kk1 Ff1 ;
ZX plane arc, U axis, Y axis linear (The J command is ignored)
(Note) Two or more axes can be designated for the linear interpolation axis.
Arc plane element speed designation
If arc plane element speed designation is selected, the F command will be handled as modal data in the same manner as the normal F command. This will also apply to the following G01, G02 and G03 commands. For example, the program will be as follows. (Example) G17 G91 G02 X10. Y10. Z-4. I10, F100 ; Helical interpolation at speed at which arc plane
element is F100 G01 X20. ; Linear interpolation at F100 G02 X10. Y-10. Z4. J10. ; Helical interpolation at speed at which arc plane
element is F100 G01 Y-40. F120 ; Linear interpolation at F120 G02 X-10. Y-10. Z-4. I10. ; Helical interpolation at speed at which arc plane
element is F120 G01 X-20. ; Linear interpolation at F120
When the arc plane element speed designation is selected, only the helical interpolation speed command is converted to the speed commanded with the arc plane element. The other linear and arc commands operate as normal speed commands. (1) The actual feedrate display (Fc) indicates the tangent element of the helical interpolation. (2) The modal value speed display (FA) indicates the command speed. (3) The speed data acquired with API functions follows the Fc and FA display. (4) This function is valid only when feed per minute (asynchronous feed: G94) is selected. If feed
per revolution (synchronous feed: G95) is selected, the arc plane element speed will not be designated.
(5) The helical interpolation option is required to use this function.
6. Interpolation Functions 6.7 Thread Cutting
56
6.7 Thread Cutting 6.7.1 Constant Lead Thread Cutting ; G33
Function and purpose
The G33 command exercises feed control over the tool which is synchronized with the spindle rotation and so this makes it possible to conduct constant-lead straight thread-cutting and tapered thread-cutting. Multiple thread screws, etc., can also be machined by designating the thread cutting angle.
Command format
G33 Z__(X__ Y__ __) F__ Q__ ; (Normal lead thread cutting commands) Z (X Y ) : Thread end point F : Lead of long axis (axis which moves most) direction Q : Thread cutting start shift angle, (0.000 to 360.000)
G33 Z__(X__ Y__ __) E__ Q__ ; (Precision lead thread cutting commands) Z (X Y ) : Thread end point E : Lead of long axis (axis which moves most) direction Q : Thread cutting start shift angle, (0.000 to 360.000)
Detailed description
(1) The E command is also used for the number of ridges in inch thread cutting, and whether the
ridge number or precision lead is to be designated can be selected by parameter setting. (Precision lead is designated by setting the parameter «#1229 set 01/bit 1» to 1.)
(2) The lead in the long axis direction is commanded for the taper thread lead.
Tapered thread section
When a<45, the lead is LZ. When a>45, the lead is LX. When a=45, the lead can be in either LX or LZ.
LZ
Z
X LX
a
6. Interpolation Functions 6.7 Thread Cutting
57
Thread cutting metric input
Input unit system B (0.001mm) C (0.0001mm)
Command address F (mm/rev) E (mm/rev) E (ridges/inch) F (mm/rev) E (mm/rev) E (ridges/inch)
Minimum command
unit
1(=1.000) (1.=1.000)
1(=1.00000) (1.=1.00000)
1(=1.00) (1.=1.00)
1(=1.0000) (1.=1.0000)
1(=1.000000) (1.=1.000000)
1(=1.000) (1.=1.000)
Command range
0.001~ 999.999
0.00001~ 999.99999
0.03~999.99 0.0001~ 999.9999
0.000001~ 999.999999
0.026~ 999.999
Input unit
system D (0.00001mm) E (0.000001mm)
Command address F (mm/rev) E (mm/rev) E (ridges/inch) F (mm/rev) E (mm/rev) E (ridges/inch)
Minimum command
unit
1(=1.00000) (1.=1.00000)
1(=1.0000000) (1.=1.0000000)
1(=1.0000) (1.=1.0000)
1(=1.000000) (1.=1.000000)
1(=1.00000000) (1.=1.00000000)
1(=1.00000) (1.=1.00000)
Command range
0.00001~ 999.99999
0.0000001~ 999.9999999
0.0255~ 999.9999
0.000001~ 999.999999
0.00000001~ 999.99999999
0.02541~ 999.99999
Thread cutting inch input
Input unit system B (0.0001inch) C (0.00001inch)
Command address F (inch/rev) E (inch/rev) E (ridges/inch) F (inch/rev) E (inch/rev) E (ridges/inch)
Minimum command
unit
1(=1.0000) (1.=1.0000)
1(=1.000000) (1.=1.000000)
1(=1.0000) (1.=1.0000)
1(=1.00000) (1.=1.00000)
1(=1.0000000) (1.=1.0000000)
1(=1.00000) (1.=1.00000)
Command range 0.0001~99.9999 0.000001~
39.370078 0.0101~
9999.9999 0.00001~ 99.99999
0.0000001~ 39.3700787
0.01001~ 9999.99999
Input unit
system D (0.000001inch) E (0.0000001inch)
Command address F (inch/rev) E (inch/rev) E (ridges/inch) F (inch/rev) E (inch/rev) E (ridges/inch)
Minimum command
unit
1(=1.000000) (1.=1.000000)
1(=1.00000000) (1.=1.00000000)
1(=1.000000) (1.=1.000000)
1(=1.0000000) (1.=1.0000000)
1(=1.000000000) (1.=1.000000000)
1(=1.0000000) (1.=1.0000000)
Command range
0.000001~ 99.999999
0.00000001~ 39.37007874
0.010001~ 9999.999999
0.0000001~ 99.9999999
0.000000001~ 39.370078740
0.0100001~ 9999.9999999
(Note 1) It is not possible to assign a lead where the feed rate as converted into per-minute
feed exceeds the maximum cutting feed rate.
(3) The constant surface speed control function should not be used for taper thread cutting commands or scrolled thread cutting commands.
(4) The thread cutting command waits for the single rotation sync signal of the rotary encoder and starts movement. Make sure to carry out timing-synchronization between part systems before issuing a thread cutting command with multiple part systems. For example, with the 1-spindle specifications with two part systems, if one part system issues a thread cutting command during ongoing thread cutting by another part system, the movement will start without waiting for the rotary encoder single rotation sync signal causing an illegal operation.
(5) The spindle speed should be kept constant throughout from the rough cutting until the finishing.
6. Interpolation Functions 6.7 Thread Cutting
58
(6) If the feed hold function is employed during thread cutting to stop the feed, the thread ridges
will lose their shape. For this reason, feed hold does not function during thread cutting. Note that this is valid from the time the thread cutting command is executed to the time the axis moves. If the feed hold switch is pressed during thread cutting, block stop will result at the end point of the block following the block in which thread cutting is completed (no longer G33 mode).
(7) The converted cutting feedrate is compared with the cutting feed clamp rate when thread cutting starts, and if it is found to exceed the clamp rate, an operation error will result.
(8) In order to protect the lead during thread cutting, a cutting feed rate which has been converted may sometimes exceed the cutting feed clamp rate.
(9) An illegal lead is normally produced at the start of the thread and at the end of the cutting because of servo system delay and other such factors. Therefore, it is necessary to command a thread length which is determined by adding the illegal lead lengths to the required thread length.
(10) The spindle speed is subject to the following restriction :
1 R Maximum feedrate Thread lead
Where R Permissible speed of encoder (r/min) R : Spindle speed (r/min) Thread lead : mm or inches Maximum feedrate : mm/min or inch/mm (This is subject to the restrictions imposed
by the machine specifications). (11) When the thread lead is extremely large to the maximum cutting feedrate enough to satisfy
«R<1» in the formula of (10) above, the program error (P93) may occur. (12) Though dry run is valid for thread cutting, the feed rate based on dry run is not synchronized
with the spindle rotation. The dry run signal is checked at the start of thread cutting and any switching during thread cutting is ignored.
(13) Synchronous feed applies for the thread cutting commands even with an asynchronous feed command (G94).
(14) Spindle override and cutting feed override are invalid and the speeds are fixed to 100% during thread cutting.
(15) When a thread cutting is commanded during tool radius compensation, the compensation is temporarily canceled and the thread cutting is executed.
(16) When the mode is switched to another automatic mode while G33 is executed, the following block which does not contain a thread cutting command is first executed and then the automatic operation stops.
(17) When the mode is switched to the manual mode while G33 is executed, the following block which does not contain a thread cutting command is first executed and then the automatic operation stops. In the case of a single block, the following block which does not contain a thread cutting command (when G33 mode is cancelled) is first executed and then the automatic operation stops. Note that automatic operation will stop immediately if the mode is switched before the G33-commanded axis starts moving.
(18) The handle interruption for automatic operation is valid while thread cutting. (19) The thread cutting start shift angle is not a modal. If there is no Q command with G33, this will
be handled as «Q0». (20) If a value more than 360.000 is commanded with G33 Q, the program error (P35) will occur. (21) G33 cuts one row with one cycle. To cut two rows, change the Q value, and issue the same
command.
6. Interpolation Functions 6.7 Thread Cutting
59
Example of program
Z
X Y
X
10 50 10
N110 G90 G0 X-200. Y-200. S50 M3 ; N111 Z110. ;
The spindle center is positioned to the workpiece center, and the spindle rotates in the forward direction.
N112 G33 Z40. F6.0 ; The first thread cutting is executed. Thread lead = 6.0mm
N113 M19 ; Spindle orientation is executed with the M19 command.
N114 G0X-210. ; The tool is evaded in the X axis direction. N115 Z110. M0 ; The tool rises to the top of the workpiece, and the
program stops with M00. Adjust the tool if required.
N116 X-200. ; M3 ;
Preparation for second thread cutting is done.
N117 G04 X5.0 ; Command dwell to stabilize the spindle rotation if necessary.
N11 G33 Z40. ; The second thread cutting is executed.
6. Interpolation Functions 6.7 Thread Cutting
60
6.7.2 Inch Thread Cutting; G33
Function and purpose
If the number of ridges per inch in the long axis direction is assigned in the G33 command, the feed of the tool synchronized with the spindle rotation will be controlled, which means that constant-lead straight thread-cutting and tapered thread-cutting can be performed.
Command format
G33 Z__ E__ Q__ ;
Z : Thread cutting direction axis address (X, Y, Z, ) and thread length E : Number of ridges per inch in direction of long axis (axis which moves
most) (decimal point command can also be assigned) Q : Thread cutting start shift angle, 0 to 360.
Detailed description
(1) The number of ridges in the long axis direction is assigned as the number of ridges per inch. (2) The E code is also used to assign the precision lead length, and whether the ridge number of
precision lead length is to be designated can be selected by parameter setting. (The number of ridges is designated by setting the parameter «#1229 set01/bit1» to 0.)
(3) The E command value should be set within the lead value range when the lead is converted. (4) The other matters are the same as uniform lead thread cutting.
6. Interpolation Functions 6.8 Unidirectional Positioning
61
Example of program
Thread lead ….. 3 threads/inch (= 8.46666 …) When programmed with 1= 10mm, 2 = 10mm using metric input
Z
X Y
X
1 50.0mm
2
N210 G90 G0X-200. Y-200. S50M3; N211 Z110.; N212 G91 G33 Z-70.E3.0; (First thread cutting) N213 M19; N214 G90 G0X-210.; N215 Z110.M0;
N216 X-200.; M3; N217 G04 X2.0; N218 G91 G33 Z-70.; (Second thread cutting)
6.8 Unidirectional Positioning; G60
Function and purpose
The G60 command can position the tool at a high degree of precision without backlash error by locating the final tool position from a single determined direction.
6. Interpolation Functions 6.8 Unidirectional Positioning
62
Command format
G60 X__ Y__ Z__ __ ; : Optional axis
Detailed description
(1) The creep distance for the final positioning as well as the final positioning direction is set by
parameter. (2) After the tool has moved at the rapid traverse rate to the position separated from the final
position by an amount equivalent to the creep distance, it move to the final position in accordance with the rapid traverse setting where its positioning is completed.
Start point
Start point End point
G60a
Stop once
Positioning position
[Final advance direction]
G60-a [G60creep distance]
+ —
(3) The above positioning operation is performed even when Z axis commands have been
assigned for Z axis cancel and machine lock. (Display only) (4) When the mirror image function is ON, the tool will move in the opposite direction as far as the
intermediate position due to the mirror image function but the operation within the creep distance during its final advance will not be affected by mirror image.
(5) The tool moves to the end point at the dry run speed during dry run when the G0 dry run function is valid.
(6) Feed during creep distance movement with final positioning can be stopped by resetting, emergency stop, interlock, feed hold and rapid traverse override zero. The tool moves over the creep distance at the rapid traverse setting. Rapid traverse override is valid.
(7) Uni-directional positioning is not performed for the drilling axis during drilling fixed cycles. (8) Uni-directional positioning is not performed for shift amount movements during the fine boring
or back boring fixed cycle. (9) Normal positioning is performed for axes whose creep distance has not been set by
parameter. (10) Uni-directional positioning is always a non-interpolation type of positioning. (11) When the same position (movement amount of zero) has been commanded, the tool moves
back and forth over the creep distance and is positioned at its original position from the final advance direction.
(12) Program error (P61) results when the G60 command is assigned with an NC system which has not been provided with this particular specification.
6. Interpolation Functions 6.9 Cylindrical Interpolation; G07.1
63
6.9 Cylindrical Interpolation; G07.1
Function and purpose
This function develops a shape with a cylindrical side (shape in cylindrical coordinate system) into a plane. When the developed shape is programmed as the plane coordinates, that is converted into the linear axis and rotation axis movement in the cylindrical coordinates and the contour is controlled during machining.
r
B
Z
X Y
As programming can be carried out with a shape with which the side on the cylinder is developed, this is effective for machining cylindrical cams, etc. When programmed with the rotation axis and its orthogonal axis, slits, etc., can be machined on the cylinder side.
Develop- ment
0
360
2r
6. Interpolation Functions 6.9 Cylindrical Interpolation; G07.1
64
Command format
G07.1 C__ ; (Cylindrical interpolation mode start/cancel) C :Cylinder radius value
Radius value 0: Cylindrical interpolation mode start Radius value = 0: Cylindrical interpolation mode cancel
(Note) The above format applies when the name of the rotation axis is «C». If the name is not «C»,
command the name of the rotation axis being used instead of «C». (1) The coordinates commanded in the interval from the start to cancellation of the cylindrical
interpolation mode will be the cylindrical coordinate system. G07.1 C Cylinder radius value; : : :
Cylindrical interpolation mode start (Cylindrical interpolation will start) (The coordinate commands in this interval will be the cylindrical coordinate system)
G07.1 C0 ; Cylindrical interpolation mode cancel (Cylindrical interpolation will be canceled)
(2) G107 can be used instead of G07.1.
6. Interpolation Functions 6.9 Cylindrical Interpolation; G07.1
65
Detailed description
(1) Command G07.1 in an independent block. A program error (P33) will occur if this command is
issued in the same block as another G code.
(2) Program the rotation axis with an angle degree.
(3) Linear interpolation or circular interpolation can be commanded during the cylindrical interpolation mode. Note that the plane selection command must be issued just before the G07.1 block.
(4) The coordinates can be commanded with either an absolute command or incremental command.
(5) Tool radius compensation can be applied on the program command. Cylindrical interpolation will be executed on the path after tool radius compensation.
(6) Command the segment feed in the cylinder development with F. The F unit is mm/min or inch/min.
(7) Cylindrical interpolation accuracy In the cylindrical interpolation mode, the movement amount of the rotation axis commanded
with an angle is converted on the circle periphery, and after operating the linear and circular interpolation between the other axes, the amount is converted into an angle again.
Thus, the actual movement amount may differ from the commanded value such as when the cylinder radius is small.
Note that the error generated at this time is not cumulated.
(8) F command during cylindrical interpolation As for the F command in the cylindrical interpolation mode, whether the previous F command
is used or not depends on that the mode just before G07.1 is the feed per minute command (G94/G98) or feed per rotation command (G95/G99).
(a) When G94 is commanded just before G07.1 If there is no F command in the cylindrical interpolation, the previous F command feedrate
will be used. The feedrate after the cylindrical interpolation mode is canceled will remain the F
command feedrate issued when the cylindrical interpolation mode was started or the final F command feedrate set during cylindrical interpolation.
(b) When G95 is commanded just before G07.1 The previous F command feedrate cannot be used during cylindrical interpolation, thus a
new F command must be issued. The feedrate after the cylindrical interpolation mode is canceled will return to that applied
before the cylindrical interpolation mode was started.
When there is no F command in G07.1 Previous mode No F command After G07.1 is canceled G94 (G98) Previous F is used G95 (G99) Program error (P62) F just before G07.1 is used
When F is commanded in G07.1
Previous mode No F command After G07.1 is canceled G94 (G98) Commanded F is used G95 (G99) Commanded F is used *1 F just before G07.1 is used
*1) Moves with the feed per minute command during G07.1.
6. Interpolation Functions 6.9 Cylindrical Interpolation; G07.1
66
(9) Plane selection The axis used for cylindrical interpolation must be set with the plane selection command.(Note) The correspondence of the rotation axis to an axis’ parallel axis is set with the parameters (#1029, #1030, #1031). The circular interpolation and tool radius compensation, etc., can be designated on that plane. The plane selection command is set immediately before or after the G07.1 command. If not set and a movement command is issued, a program error (P485) will occur.
(Example)
Basic coordinate system X, Y, Z
Cylindrical coordinate system C, Y, Z (Rotation axis is X axis’ parallel axis) #1029
Cylindrical coordinate system X, C, Z (Rotation axis is Y axis’ parallel axis) #1030
Cylindrical coordinate system X, Y, C (Rotation axis is Z axis’ parallel axis) #1031
G17
Y
X
G18
Z
X
G19
Y
Z
G18
Z
C
G18
C
X
G19
C
Z
G19
Y
C
G17
X
C
G17
C
Y
G19 Z0. C0. ;
G07.1 C100. ;
:
G07.1 C0 ;
(Note) Depending on the model or version, the Z-C plane (Y-Z cylinder plane) will be automatically
selected with G07.1 and G19. The circular interpolation and tool radius compensation, etc., can be designated on that
plane.
Basic coordinate system X, Y, Z
Cylindrical coordinate system
G17
Y
X
G18
Z
X
G19
Y
Z
G19
Z
C
6. Interpolation Functions 6.9 Cylindrical Interpolation; G07.1
67
(10) Related parameters
# Item Details Setting range
1516 mill_ax Milling axis name
Set the name of the rotation axis for milling interpolation (pole coordinate interpolation, cylindrical interpolation). Only one of the rotation axes can be set.
A to Z
8111 Milling Radius Select the diameter and radius of the linear axis for milling interpolation (pole coordinate interpolation, cylindrical interpolation). 0: Radius command for all axes 1: Each axis setting (follows #1019 dia diameter
designation axis)
0 / 1
1267 (PR)
ext03 (bit0)
G code type The type of G code is changed. 0: Conventional format 1: Mitsubishi special format
0 / 1
1270 (PR)
ext06 (bit7)
Handle C axis coordinate during cylindrical interpolation
Specify whether the rotary axis coordinate before the cylindrical interpolation start command is issued is kept during the cylindrical interpolation or not. 0: Do not keep 1: keep
0 / 1
Relation with other functions
(1) The following G code commands can be used during the cylindrical interpolation
mode. G code Details
G00 G01 G02 G03 G04 G09 G40-42 G61 G64 G65 G66 G66.1 G67 G80-89 G90/91 G94 G98 G99
Positioning Linear interpolation Circular interpolation (CW) Circular interpolation (CWW) Dwell Exact stop check Tool nose R compensation Exact stop check mode Cutting mode Macro call (simple call) Macro modal call A (modal call) Macro modal call B (block call per macro) Macro modal call cancel (modal call cancel) Hole drilling fixed cycle Absolute/incremental value command Asynchronous feed Hole drilling cycle initial return Hole drilling cycle R point return
A program error (P481) may occur if a G code other than those listed above is commanded during cylindrical interpolation.
(2) Circular interpolation
(a) Circular interpolation between the rotation axis and linear axis is possible during the cylindrical interpolation mode.
(b) An R specification command can be issued with circular interpolation. (I, J and K cannot be designated.)
6. Interpolation Functions 6.9 Cylindrical Interpolation; G07.1
68
(3) Tool radius compensation The tool radius can be compensated during the cylindrical interpolation mode.
(a) Command the plane selection in the same manner as circular interpolation. When using tool radius compensation, start up and cancel the compensation within the
cylindrical interpolation mode.
(b) A program error (P485) will occur if G07.1 is commanded during tool radius compensation.
(c) If the G07.1 command is issued with no movement command given after the tool radius compensation is canceled, the position of the axis in the G07.1 command block is interpreted as the position applied after the tool radius compensation is canceled and the following operations are performed.
(4) Tool length compensation
(a) A program error (P481) will occur if the tool length compensation is carried out in the cylindrical interpolation mode. : : G43H12 ; … Tool length compensation before cylindrical interpolation Valid G0 X100. Z0 ; G19 Z C ; G07.1 C100. ; : G43H11 ; … Tool length compensation in cylindrical interpolation mode Program error : G07.1 C0 ;
(b) Complete the tool compensation movement (movement of tool length and wear compensation amount) before executing the cylindrical interpolation. If the tool compensation movement is not completed when the cylindrical interpolation start command has been issued, the followings will be resulted: Machine coordinate is not changed even if G07.1 is executed.
The workpiece coordinate is changed to that of the post tool length compensation when G07.1 is executed. (Even if canceling the cylindrical interpolation, this workpiece coordinate will not be canceled.)
(5) Cutting asynchronous feed
(a) The asynchronous mode is forcibly set when the cylindrical interpolation mode is started.
(b) When the cylindrical interpolation mode is canceled, the synchronization mode will return to the state before the cylindrical interpolation mode was started.
(c) A program error (P485) will occur if G07.1 is commanded in the constant surface speed control mode (G96).
(6) Miscellaneous functions
(a) The miscellaneous function (M) and 2nd miscellaneous function can be issued even in the cylindrical interpolation mode.
(b) The S command in the cylindrical interpolation mode issues the rotary tool’s rotation speed instead of the spindle rotation speed.
6. Interpolation Functions 6.9 Cylindrical Interpolation; G07.1
69
Restrictions and precautions
(1) The cylindrical interpolation mode is canceled when the power is turned ON or reset.
(2) A program error (P484) will occur if any axis commanded for cylindrical interpolation has not completed reference position return.
(3) Tool radius compensation must be canceled before the cylindrical interpolation mode can be canceled.
(4) When the cylindrical interpolation mode is canceled, the mode will change to the cutting mode, and the plane will return to that selected before cylindrical interpolation.
(5) The program of the block during the cylindrical interpolation cannot be restarted (program restart).
(6) A program error (P486) will occur if the cylindrical interpolation command is issued during the mirror image.
(7) When the cylindrical interpolation mode is started or canceled, the deceleration check is performed.
(8) A program error (P481) will occur if the cylindrical interpolation or the pole coordinate interpolation is commanded during the cylindrical interpolation mode.
6. Interpolation Functions 6.9 Cylindrical Interpolation; G07.1
70
Example of program
#1029 aux_I #1030 aux_J C #1031 aux_K
Command of plane selection for cylindrical interpolation and command of two interpolation axes Cylindrical interpolation start Cylindrical interpolation cancel
N01 G28XZC; N02 G97S100M23; N03 G00X50.Z0.; N04 G94G01X40.F100.; N05 G19C0Z0; N06 G07.1C20.; N07 G41; N08 G01Z-10.C80.F150; N09 Z-25.C90.; N10 Z-80.C225; N11 G03Z-75.C270.R55.; N12 G01Z-25; N13 G02Z-20.C280.R80.; N14 G01C360. N15 G40; N16 G07.1C0; N17 G01X50.; N18 G0X100.Z100.; N19 M25; N20 M30;
(Unit: mm)
50
100
150
200
250
300
350
-20-40-60-80
C
Z
N09 N10
N11
N12 N13
N14
N15
N11
10
09 N08
N13
N14
N12
6. Interpolation Functions 6.10 Polar Coordinate Interpolation; G12.1, G13.1/G112,G113
71
6.10 Polar Coordinate Interpolation; G12.1, G13.1/G112,G113
Function and purpose
This function converts the commands programmed with the orthogonal coordinate axis into linear axis movement (tool movement) and rotation axis movement (workpiece rotation), and controls the contour. The plane that uses the linear axis as the plane’s 1st orthogonal axis, and the intersecting hypothetical axis as the plane’s 2nd axis (hereafter «pole coordinate interpolation plane») is selected. Pole coordinate interpolation is carried out on this plane. The workpiece coordinate system zero point is used as the coordinate system zero point during pole coordinate interpolation.
Linear axis
X axis
C axis
Z axis
Rotation axis (hypothetical axis)
Polar coordinate interpolation plane (G17 plane)
This is effective for cutting a notch section on a linear section of the workpiece diameter, and for cutting cam shafts, etc.
Command format
G12.1 ; Pole coordinate interpolation mode start G13.1 ; Pole coordinate interpolation mode cancel
(1) The coordinates commanded in the interval from the start to cancellation of the pole
coordinate interpolation mode will be the pole coordinate interpolation. G12.1 ; Pole coordinate interpolation mode start : (Pole coordinate interpolation will start) : (The coordinate commands in this interval will be the pole coordinate : interpolation) G13.1 ; Pole coordinate interpolation mode cancel (Pole coordinate interpolation is canceled)
(2) G112 and G113 can be used instead of G12.1 and G13.1.
6. Interpolation Functions 6.10 Polar Coordinate Interpolation; G12.1, G13.1/G112,G113
72
Detailed description
(1) Command G12.1 and G13.1 in an independent block. A program error (P33) will occur if this
command is issued in the same block as another G code.
(2) Linear interpolation or circular interpolation can be commanded during the pole coordinate interpolation mode.
(3) The coordinates can be commanded with either an absolute command or incremental command.
(4) Tool radius compensation can be applied on the program command. Pole coordinate interpolation will be executed on the path after tool radius compensation.
(5) Command the segment feed in the pole coordinate interpolation plane (orthogonal coordinate system) with F. The F unit is mm/min or inch/min.
(6) When the G12.1 command is issued, the deceleration check is executed.
(7) Plane selection The linear axis and rotation axis used for pole coordinate interpolation must be set beforehand
with the parameters.
(a) Determine the deemed plane for carrying out pole coordinate interpolation with the parameter (#1533) for the linear axis used for pole coordinate interpolation.
#1533 setting value Deemed plane X G17 (XY plane) Y G19 (YZ plane) Z G18 (ZX plane)
Blank (no setting) G17 (XY plane)
(b) A program error (P485) will occur if the plane selection command (G16 to G19) is issued during the pole coordinate interpolation mode.
(Note) Depending on the model or version, parameter (#1533) may not be provided. In this case, the operation will be the same as if the parameter (#1533) is blank (no setting).
6. Interpolation Functions 6.10 Polar Coordinate Interpolation; G12.1, G13.1/G112,G113
73
(8) F command during pole coordinate interpolation As for the F command in the pole coordinate interpolation mode, whether the previous F command is used or not depends on that the mode just before G12.1 is the feed per minute command (G94/G98) or feed per rotation command (G95/G99).
(a) When G94(G98) is commanded just before G12.1 If there is no F command in the pole coordinate interpolation, the previous F command feedrate will be used. The feedrate after the pole coordinate interpolation mode is canceled will remain the F command feedrate issued when the pole coordinate interpolation mode was started or the final F command feedrate set during pole coordinate interpolation. The previous F command feedrate cannot be used during pole coordinate interpolation.
(b) When G95(G99) is commanded just before G12.1 The previous F command feedrate cannot be used during pole coordinate interpolation. A new F command must be issued. The feedrate after the pole coordinate interpolation mode is canceled will return to that applied before the pole coordinate interpolation mode was started.
When there is no F command in G12.1
Previous mode No F command After G13.1 is canceled G94(G98) Previous F is used G95(G99) Program error (P62) F just before G12.1 is used
When F is commanded in G12.1
Previous mode No F command After G07.1 is canceled G94(G98) Commanded F is used G95(G99) Commanded F is used *1 F just before G12.1 is used
*1) Moves with the feed per minute command during G12.1.
(9) Related parameters
# Item Details Setting range
1516 mill_ax Milling axis name
Set the name of the rotation axis for milling interpolation (pole coordinate interpolation, cylindrical interpolation). Only one of the rotation axes can be set.
A to Z
1517 mill_c Milling interpolation hypothetical axis name
Select the hypothetical axis command name for milling interpolation (pole coordinate interpolation, cylindrical interpolation). 0: Y axis command 1: Command rotation axis name
0 / 1
8111 Milling Radius Select the diameter and radius of the linear axis for milling interpolation. 0: Radius command for all axes 1: Each axis setting (follows #1019 dia diameter
designation axis)
0 / 1
1533 mill_Pax Polar coordinate linear axis name
Set the linear axis for polar coordinate interpolation. Axis name
6. Interpolation Functions 6.10 Polar Coordinate Interpolation; G12.1, G13.1/G112,G113
74
Relation with other functions
(1) The following G code commands can be used during the pole coordinate interpolation mode.
G code Details G00 G01 G02 G03 G04 G09 G40-42 G61 G64 G65 G66 G66.1 G67 G80-89 G90/91 G94 G98 G99
Positioning Linear interpolation Circular interpolation (CW) Circular interpolation (CWW) Dwell Exact stop check Tool radius compensation Exact stop check mode Cutting mode Macro call (simple call) Macro modal call A (modal call) Macro modal call B (block call per macro) Macro modal call cancel (modal call cancel) Hole drilling fixed cycle Absolute/incremental value command Asynchronous feed Hole drilling cycle initial return Hole drilling cycle R point return
A program error (P481) may occur if a G code other than those listed above is commanded during pole coordinate interpolation.
(2) Program commands during pole coordinate interpolation
(a) The program commands in the pole coordinate interpolation mode are commanded with the orthogonal coordinate value of the linear axis and rotation axis (hypothetical axis) on the pole coordinate interpolation plane.
The axis address of the rotation axis (C) is commanded as the axis address for the plane’s 2nd axis (hypothetical axis) command.
The command unit is not degree, and instead is the same unit (mm or inch) as the command issued with the axis address for the plane’s 1st axis (linear axis).
(b) The hypothetical axis coordinate value will be set to «0» when G12.1 is commanded. In other words, the position where G12.1 is commanded will be interpreted as angle = 0, and the pole coordinate interpolation will start.
(3) Circular interpolation on pole coordinate plane The arc radius address for carrying out circular interpolation during the pole coordinate
interpolation mode is determined with the linear axis parameter (#1533). #1533 setting value Center designation command
X I, J (pole coordinate plane is interpreted as XY plane) Y J, K (pole coordinate plane is interpreted as YZ plane) Z K, I (pole coordinate plane is interpreted as ZX plane)
Blank (no setting) I, J (pole coordinate plane is interpreted as XY plane)
The arc radius can also be designated with the R command.
(Note) Depending on the model or version, parameter (#1533) may not be provided. In this case, the operation will be the same as if the parameter (#1533) is blank (no setting).
6. Interpolation Functions 6.10 Polar Coordinate Interpolation; G12.1, G13.1/G112,G113
75
(4) Tool radius compensation The tool radius can be compensated during the pole coordinate interpolation mode.
(a) Command the plane selection in the same manner as pole coordinate interpolation. When using tool radius compensation, it must be started up and canceled within the pole
coordinate interpolation mode.
(b) A program error (P485) will occur if polar coordinate interpolation is executed during tool radius compensation.
(c) If the G12.1 and G13.1 commands are issued with no movement command given after the tool radius compensation is canceled, the position of the axis in the G12.1 and G13.1 commands block is interpreted as the position applied after the tool radius compensation is canceled and the following operations are performed.
(5) Tool length compensation
(a) A program error (P481) will occur if the tool length compensation is carried out in the polar coordinate interpolation mode.
: : G43 H12 ; …Tool length compensation before polar coordinate interpolation Valid G0 X100. Z0 ; G12.1 ; : G43 H11 ; …Tool length compensation in polar coordinate interpolation mode
Program error : G13.1 ;
(b) Complete the tool compensation operation (movement of tool length and wear compensation amount) before executing the polar coordinate interpolation. If the tool compensation operation is not completed when the polar coordinate interpolation start command has been issued, the followings will be resulted:
Machine coordinate is not changed even if G12.1 is executed..
The workpiece coordinate is changed to that of the post tool length compensation when G12.1 is executed. (Even if canceling the polar coordinate interpolation, this workpiece coordinate will not be canceled.)
(6) Cutting asynchronous feed
(a) The asynchronous mode is forcibly set when the pole coordinate interpolation mode is started.
(b) When the pole coordinate interpolation mode is canceled, the synchronization mode will return to the state before the pole coordinate interpolation mode was started.
(c) A program error (P485) will occur if G12.1 is commanded in the constant surface speed control mode (G96).
(7) Miscellaneous functions
(a) The miscellaneous function (M) and 2nd miscellaneous function can be issued even in the pole coordinate interpolation mode.
(b) The S command in the pole coordinate interpolation mode issues the rotary tool’s rotation speed instead of the spindle rotation speed.
6. Interpolation Functions 6.10 Polar Coordinate Interpolation; G12.1, G13.1/G112,G113
76
(8) Hole drilling axis in the hole drilling fixed cycle command during the pole coordinate
interpolation Hole drilling axis in the hole drilling fixed cycle command during the pole coordinate interpolation is determined with the linear axis parameter (#1533).
#1533 setting value Hole drilling axis X Z (pole coordinate plane is interpreted as XY plane) Y X (pole coordinate plane is interpreted as YZ plane) Z Y (pole coordinate plane is interpreted as ZX plane)
Blank (no setting) Z (pole coordinate plane is interpreted as XY plane)
(9) Shift amount in the G76 (fine boring) or G87 (back boring) command during the pole coordinate interpolation
Shift amount in the G76 (fine boring) or G87 (back boring) command during the pole coordinate interpolation is determined with the linear axis parameter (#1533).
#1533 setting value Center designation command X I, J (pole coordinate plane is interpreted as XY plane) Y J, K (pole coordinate plane is interpreted as YZ plane) Z K, I (pole coordinate plane is interpreted as ZX plane)
Blank (no setting) I, J (pole coordinate plane is interpreted as XY plane)
Restrictions and precautions
(1) The program cannot be restarted (resumed) for a block in pole coordinate interpolation.
(2) Before commanding pole coordinate interpolation, set the workpiece coordinate system so that the center of the rotation axis is at the coordinate system zero point. Do not change the coordinate system during the pole coordinate interpolation mode. (G50, G52, G53, relative coordinate reset, G54 to G59, etc.)
(3) The feedrate during pole coordinate interpolation will be the interpolation speed on the pole coordinate interpolation plane (orthogonal coordinate system). (The relative speed with the tool will be converted with pole coordinate conversion.) When passing near the center of the rotation axis on the pole coordinate interpolation plane (orthogonal coordinate system), the rotation axis side feedrate after pole coordinate interpolation will be very high.
(4) The axis movement command outside of the plane during pole coordinate interpolation will move unrelated to the pole coordinate interpolation.
(5) The current position displays during pole coordinate interpolation will all indicate the actual coordinate value. However, the «remaining movement amount» will be the movement amount on the pole coordinate input plane.
(6) The pole coordinate interpolation mode will be canceled when the power is turned ON or reset.
(7) A program error (P484) will occur if any axis commanded for pole coordinate interpolation has not completed zero point return.
(8) Tool radius compensation must be canceled before the pole coordinate interpolation mode can be canceled.
(9) When the pole coordinate interpolation mode is canceled, the mode will change to the cutting mode, and the plane will return to that selected before pole coordinate interpolation.
(10) A program error (P486) will occur if the pole coordinate interpolation command is issued during the mirror image.
6. Interpolation Functions 6.10 Polar Coordinate Interpolation; G12.1, G13.1/G112,G113
77
(11) A program error (P486) will occur if the cylindrical interpolation or the pole coordinate interpolation is commanded during the pole coordinate interpolation mode.
(12) During pole coordinate interpolation, if X axis moveable range is controlled in the plus side, X axis has to be moved to the plus area that includes «0» and above before issuing the polar coordinate interpolation command. If X axis moveable range is controlled in the minus side, X axis has to be moved to the area that does not include «0» before issuing the polar coordinate interpolation command.
Example of program
Hypothetical C axis
X axis
Z axis
C axis
Hypothetical C axis
C axis
Tool
X axis
N01 N02
N11
N05
N04
N03
N10
N09 N08
N07
N06
Path after tool radius compensation Program path
: N01 G17 G90 G0 X40.0 C0 Z0; N02 G12.1; N03 G1 G42 X20.0 F2000; N04 C10.0; N05 G3 X10.0 C20.0 R10.0; N06 G1 X-20.0; N07 C-10.0; N08 G3 X-10.0 C-20.0 I10.0 J0; N09 G1 X20.0; N10 C0; N11 G40 X40.0; N12 G13.1; : : M30 ;
Setting of start position Polar coordinate interpolation mode: Start Actual machining start Shape program (Command the position with the orthogonal coordinate on X-C hypothetical axis plane.) Polar coordinate interpolation mode: Cancel
6. Interpolation Functions 6.11 Exponential Function Interpolation; G02.3, G03.3
78
6.11 Exponential Function Interpolation; G02.3, G03.3
Function and purpose
Exponential function interpolation changes the rotation axis into an exponential function shape in respect to the linear axis movement. At this time, the other axes carry out linear interpolation between the linear axis. This allows a machining of a taper groove with constant torsion angle (helix angle) (uniform helix machining of taper shape). This function can be used for slotting or grinding a tool for use in an end mill, etc. Uniform helix machining of taper shape
(Linear axis)
Torsion angle: J1=J2=J3
A axis (Rotation axis)
Z axis
X axis
J1
J2
J3
(G02.3/G03.3)
(G00)
(G01) (G01)
Relation of linear axis and rotation axis
A axis (Rotation axis)
«Relation of linear axis and rotation axis»
X=B (eCA-1) {B, C … constant}
X axis (Linear axis)
6. Interpolation Functions 6.11 Exponential Function Interpolation; G02.3, G03.3
79
Command format
G02.3/G03.3 Xx1 Yy1 Zz1 Ii1 Jj1 Rr1 Ff1 Qq1 Kk1 ; G02.3 : Forward rotation interpolation (modal) G03.3 : Negative rotation interpolation (modal) X : X axis end point (Note 1) Y : Y axis end point (Note 1) Z : Z axis end point (Note 1) I : Angle i1 (Note 2) J : Angle j1 (Note 2) R : Constant value r1 (Note 3) F : Initial feedrate (Note 4) Q : Feedrate at end point (Note 5) K : Command will be ignored.
(Note 1) Designate the end point of the linear axis designated with parameter «#1514 expLinax» and the axis that carries out linear interpolation between that axis.
If the end point on of the rotation axis designated with parameter «#1515 expRotax» is designated, linear interpolation without exponential function interpolation will take place.
(Note 2) The command unit is as follows.
Setting unit #1003 = B #1003 = C #1003 = D #1003 = E (Unit = ) 0.001 0.0001 0.00001 0.000001
The command range is -89 to +89. A program error (P33) will occur if there is no address I or J command. A program error (P35) will occur if the address I or J command value is 0. (Note 3) The command unit is as follows.
Setting unit #1003 = B #1003 = C #1003 = D #1003 = E Unit Metric system 0.001 0.0001 0.00001 0.000001 mm Inch system 0.0001 0.00001 0.000001 0.0000001 inch
The command range is a positive value that does not include 0. A program error (P33) will occur if there is no address R command. A program error (P35) will occur if the address R command value is 0. (Note 4) The command unit and command range is the same as the normal F code. (Command
as a per minute feed.) Command the composite feedrate that includes the rotation axis. The normal F modal value will not change by the address F command. A program error (P33) will occur if there is no address F command. A program error (P35) will occur if the address F command value is 0.
6. Interpolation Functions 6.11 Exponential Function Interpolation; G02.3, G03.3
80
(Note 5) The command unit is as follows.
Setting unit #1003 = B #1003 = C #1003 = D #1003 = E Unit Metric system 0.001 0.0001 0.00001 0.000001 mm Inch system 0.0001 0.00001 0.000001 0.0000001 inch
The command unit and command range is the same as the normal F code. Command the composite feedrate that includes the rotation axis. The normal F modal value will not change by the address Q command. The axis will interpolate between the initial speed (F) and end speed (Q) in the CNC
according to the linear axis. If there is no address Q command, interpolation will take place with the same value as
the initial feedrate (address F command). (The start point and end point feedrates will be the same.)
A program error (P35) will occur if the address Q command value is 0.
Example of uniform helix machining of taper shape
i1
j1 x1 x0
r1
Z axis Z axis
A axis
Linear axis … X axis, rotation axis … A axis, linear axis (X axis) start point … x0
X axis
Relational expression of exponential function
The exponential function relational expression of the linear axis (X) and rotation axis (A) in the G02.3/G03.3 command is defined in the following manner. X () = r1 (e/D- 1) / tan (i1) (linear axis (X) movement (1)) A () = (-1) 360 / (2) (rotation axis (A) movement) D = tan (j1) / tan (i1) = 0 during forward rotation (G02.3), and = 1 during reverse rotation (G03.3) is the rotation angle (radian) from the rotation axis’ start point The rotation axis’ rotation angle () is as follows according to expression (1). = D 1n { (X tan (i1) / r1) + 1 }
6. Interpolation Functions 6.11 Exponential Function Interpolation; G02.3, G03.3
81
Machining example
Example of uniform helix machining of taper shape
i1
j1 x1 x0 x2
p1
A axis
r1 r2
z1 z2 z0
X axis
Z axis
Z () = r1 (e/D-1) tan (p1) / tan (i1) + z0 … (1) X () = r1 (e/D-1) / tan (i1) … (2) A () = (-1) 360 / (2) D = tan (j1) / tan (i1) Z () Absolute value from zero point of Z axis (axis that linearly interpolates between interval
with linear axis (X axis)) X () Absolute value from X axis (linear axis) start point A () Absolute value from A axis (rotation axis) start point r1 Exponential function interpolation constant value (address R command) r2 Workpiece left edge radius x2 X axis (linear axis) position at workpiece left edge x1 X axis (linear axis) end point (address X command) x0 X axis (linear axis) start point (Set as «x0 x1» so that workpiece does not interfere with
tool) z1 End point of Z axis (axis that linearly interpolates between interval with linear axis (X
axis)) (address Z command) z0 Start point of Z axis (axis that linearly interpolates between interval with linear axis (X
axis)) i1 Taper gradient angle (address I command) p1 Slot base gradient angle j1 Torsion angle (helix angle) (address J command) Torsion direction (0: Forward rotation, 1: reverse direction) Workpiece rotation angle (radian) f1 Initial feedrate (address F command) q1 Feedrate at end point (address Q command) k1 Insignificant data (address K command) According to expressions (1) and (2): Z () = X () tan (p1) + z0 … (3) According to expression (3), the slot base gradient angle (p1) is determined from the X axis and Z axis end point positions (x1, z1). The Z axis movement amount is determined by the slot base gradient angle (p1) and X axis position. In the above diagram, the exponential function interpolation’s constant value (r1) is determined with the following expression using the workpiece left edge radius (r2), X axis start point (x0), X axis position at workpiece left edge (x2) and taper gradient angle (i1). r1 = r2 — { (x2 — x0) tan (i1) } … (4)
6. Interpolation Functions 6.11 Exponential Function Interpolation; G02.3, G03.3
82
The taper gradient angle (i1) and torsion angle (j1) are each issued with the command address I and J. Note that if the shape is a reverse taper shape, the taper gradient angle (i1) is issued as a negative value. The torsion direction () is changed with the G code. (Forward rotation when G02.3 is commanded, negative rotation when G03.3 is commanded) The above settings allow uniform helix machining of a taper shape (or reverse taper shape).
Command and operation
G2.3(Equivalent to G3.3 if j1<0)
X movement direction > 0 X movement direction < 0
i1>0 i1<0 i1>0 i1<0
C om
m an
d
i1
X
Z End point
j1
r1
Start point
—
X
Z +
j1
i1
r1
End point
Start point
X
Z
j1
i1
r1
Start point
End point
End point
Start point
X
Z+ —
j1
i1
r1
O pe
ra tio
n
X
A
X
A
X
A
X
A
M ac
hi ni
ng
pr og
ra m
e xa
m pl
e N10 G28XYZC;
N20 G91G0 X100. Z100.;
N30 G2.3 X100. Z100.
I50. J80. R105. F500.;
N40 M30;
N10 G28XYZC;
N20 G91G0 X100. Z200.;
N30 G2.3 X100. Z-100.
I-50. J80. R105. F500.;
N40 M30;
N10 G28XYZC;
N20 G91G0 X-100. Z100.;
N30 G2.3 X-100. Z100.
I50. J80. R105. F500.;
N40 M30;
N10 G28XYZC;
N20 G91G0 X-100. Z200.;
N30 G2.3 X-100. Z-100.
I-50. J80. R105. F500.;
N40 M30;
G3.3(Equivalent to G2.3 if j1<0)
X movement direction > 0 X movement direction < 0
i1>0 i1<0 i1>0 i1<0
C om
m an
d
End point Start
point
X
Z
j1
i1
r1
End point
Start point
—
X
Z +
j1
r1
Start point
End point
X
Z
j1
i1
r1
End point
Start point
X
Z+ —
j1
i1
r1
O pe
ra tio
n
X A
X
A
X A
X
A
M ac
hi ni
ng
pr og
ra m
e xa
m pl
e N10 G28XYZC;
N20 G91G0 X100. Z100.;
N30 G3.3 X100. Z100.
I50. J80. R105. F500.;
N40 M30;
N10 G28XYZC;
N20 G91G0 X100. Z200.;
N30 G3.3 X100. Z-100.
I-50. J80. R105. F500.;
N40 M30;
N10 G28XYZC;
N20 G91G0 X-100. Z100.;
N30 G3.3 X-100. Z100.
I50. J80. R105. F500.;
N40 M30;
N10 G28XYZC;
N20 G91G0 X-100. Z200.;
N30 G3.3 X-100. Z-100.
I-50. J80. R105. F500.;
N40 M30;
6. Interpolation Functions 6.11 Exponential Function Interpolation; G02.3, G03.3
83
Precautions for programming
(1) When G02.3/G03.3 is commanded, interpolation takes place with the exponential function
relational expression using the start position of the linear axis and rotation axis as 0.
(2) Linear interpolation will take place in the following cases, even if in the G02.3/G03.3 mode. The feedrate for linear interpolation will be the F command in that block. (Note that the normal
F modal is not updated.) The linear axis designated with the parameter (#1514 expLinax) is not commanded, or the
movement amount for that axis is 0. The rotation axis designated with the parameter (#1515 expRotax) is commanded.
(3) A program error will occur if the following commands are issued in G02.3 or G03.3 mode. A program error will also occur if G02.3 or G03.3 command is issued in the following modes.: Tool length compensation
(A program error will occur only when the compensation starts at the same time as the movement by exponential function interpolation. The tool length compensation will operate normally if it has started before the G02.3/G03.3 mode starts.
Tool radius compensation High-speed high-accuracy control High-speed machining Scaling Tool length compensation along tool axis Figure rotation Coordinate rotation by program Coordinate rotation by parameter 3-dimentional coordinate conversion
(4) A program error (P481) will occur if commands are issued during the pole coordinate interpolation, cylindrical interpolation or milling interpolation modes.
(5) Program error (P612) will occur if commands are issued during the scaling or mirror image.
(6) Program error (P34) will occur if commands are issued during the high-speed high-accuracy control II.
(7) G02.3/G03.3 will function with asynchronous feed even during the synchronous feed mode.
(8) If the parameter «#1515 expRota» setting is the same axis name as the initial C axis, the axis selected with the C axis selection signal will interpolate as the rotation axis.
6. Interpolation Functions 6.12 Polar Coordinate Command ; G16/G15
84
6.12 Polar Coordinate Command ; G16/G15
Function and purpose
With this function, the end point coordinate value is commanded with the polar coordinate of the radius and angle.
Command format
G16 ; Polar coordinate command mode ON G15 ; Polar coordinate command mode OFF
Detailed description
(1) The polar coordinate command is applied in the interval from turning ON to OFF of the polar
coordinate command mode. G1x ; G16 ;
Plane selection for polar coordinate command (G17/G18/G19) Polar coordinate command mode ON
G9x G01 Xx1 Yy1 F2000 ; :
Polar coordinate command G9x : Center selection for polar coordinate command (G90/G91)
G90 The workpiece coordinate system zero point is the polar coordinate center.
G91 The present position is the polar coordinate center. x1 : 1st axis for the plane The radius commanded y1 : 2nd axis for the plane The angle commanded
For G90/G17(X-Y plane)
Commanded position
Present position y1
x1
X
Y
Plus
Minus
G15 ;
Polar coordinate command mode OFF
(2) The plane selection during the polar coordinate command mode is carried out with G17, G18 and G19.
(3) The polar coordinate command is a modal. The polar coordinate command mode when the power is turned ON is OFF (G15). Whether to initialize the modal at reset or not can be selected with the parameter (#1210 RstGmd/bit 11) setting.
(4) During polar coordinate command mode, command the radius with the 1st axis for the selected plane, and the angle with the 2nd axis. For example, when the X-Y plane is selected, command the radius with the address «X», and the angle with the address «Y».
(5) For the angle, the counterclockwise direction of the selected plane is positive and the clockwise direction is negative.
(6) The radius and angle can be commanded with both the absolute value and incremental value (G90, G91).
6. Interpolation Functions 6.12 Polar Coordinate Command ; G16/G15
85
(7) When the radius is commanded with the absolute value, command the distance from the zero
point in the workpiece coordinate system (note that the local coordinate system is applied when the local coordinate system is set).
(8) When the radius is commanded with the incremental value command, considering the end point of the previous block as the polar coordinate center, command the incremental value from that end point. The angle is commanded with the incremental value of the angle from the previous block.
(9) When the radius is commanded with the negative value, the same operation as the command that the radius command value is changed to the absolute value and 180 is added to the angle command value.
Command position
(1) When the zero point in the workpiece coordinate system is applied to the polar
coordinate center The zero point in the workpiece coordinate system is applied to the polar coordinate center by
commanding the radius with the absolute value. Note that the zero point in the local coordinate system is applied to the polar coordinate center if the local coordinate system (G52) is used.
When the angle is the absolute value command
When the angle is the incremental value command
Command position
Present position
Angle
Radius
Command position
Present position Angle
Radius
Command position when the zero point in the workpiece coordinate system is applied to the polar coordinate center
(2) When the present position is applied to the polar coordinate center The present position is applied to the polar coordinate center by commanding the radius with
the incremental value.
When the angle is the absolute value command
When the angle is the incremental value command
Command position
Present position
Angle
Radius
Command position
Present position
Angle Radius
Command position when the present position is applied to the polar coordinate center
6. Interpolation Functions 6.12 Polar Coordinate Command ; G16/G15
86
(3) When the radius command is omitted When the radius command is omitted, the zero point in the workpiece coordinate system is
applied to the polar coordinate center, and the distance between the polar coordinate center and current position is regarded as the radius. Note that the zero point in the local coordinate system is applied to the polar coordinate center if the local coordinate system (G52) is used.
When the angle is the absolute value command
When the angle is the incremental value command
Command position
Present position Angle
Present position Angle
Radius
Command position
Radius
Command position when the radius command is omitted
(4) When the angle command is omitted When the angle command is omitted, the angle of the present position in the workpiece
coordinate system is applied to the angle command. The zero point in the workpiece coordinate system is applied to the polar coordinate center by commanding the radius with the absolute value. Note that the zero point in the local coordinate system is applied to the polar coordinate center if the local coordinate system (G52) is used. If the radius is commanded with the incremental value, the present position is applied to the polar coordinate center.
When the radius is the absolute value command
When the radius is the incremental value command
Command position
Present position
Radius
Angle
Command position
Present position
Radius
Angle
Command position when the angle command is omitted
6. Interpolation Functions 6.12 Polar Coordinate Command ; G16/G15
87
Axis command not interpreted as polar coordinate command
The axis command with the following command is not interpreted as the polar coordinate command during the polar coordinate command mode. The movement command that has no axes commands for the 1st axis and 2nd axis in the selected plane mode is also not interpreted as polar coordinate command during the polar coordinate command mode.
Function G code Dwell G04 Program parameter input/compensation input
G10
Local coordinate system setting G52 Machine coordinate system setting G92 Machine coordinate system selection G53 Coordinate rotation by program G68 Scaling G51 G command mirror image G51.1 Reference position check G27 Reference position return G28 Start position return G29 2nd to 4th reference position return G30 Tool change position return 1 G30.1 Tool change position return 2 G30.2 Tool change position return 3 G30.3 Tool change position return 4 G30.4 Tool change position return 5 G30.5 Tool change position return 6 G30.6 Automatic tool length measurement G37 Skip G31 Multi-step skip function 1-1 G31.1 Multi-step skip function 1-2 G31.2 Multi-step skip function 1-3 G31.2 Linear angle command G01 Aa1
6. Interpolation Functions 6.12 Polar Coordinate Command ; G16/G15
88
Example of program
When the zero point in the workpiece coordinate system is the polar coordinate zero point
The polar coordinate zero point is the zero point in the workpiece coordinate system.
The plane is the X-Y plane.
200mm
X
Y
30
120
270
N4
N2
N3
(1) When the radius and angle are the absolute value command
N1 G17 G90 G16 ; Polar coordinate command, X-Y plane selection The polar coordinate zero point is the zero point
in the workpiece coordinate system. N2 G85 X200. Y30. Z-20. F200. ; Radius 200mm, angle 30 N3 Y120. ; Radius 200mm, angle 120 N4 Y270. ; Radius 200mm, angle 270 N5 G15 G80 ; Polar coordinate command cancel
(2) When the radius is the absolute value command and the angle is the incremental value
command N1 G17 G90 G16 ;
Polar coordinate command, X-Y plane selection The polar coordinate zero point is the zero point in the workpiece coordinate system.
N2 G85 X200. Y30. Z-20. F200. ; Radius 200mm, angle 30 N3 G91 Y90. ; Radius 200mm, angle + 90 N4 Y150. ; Radius 200mm, angle +150 N5 G15 G80 ; Polar coordinate command cancel
6. Interpolation Functions 6.12 Polar Coordinate Command ; G16/G15
89
Precautions
(1) If the following commands are carried out during the polar coordinate command mode, or if the
polar coordinate command is carried out during the following command mode, a program error (P34) will occur.
Function G code High-speed high-accuracy control I
G05.1 Q1
High-speed high-accuracy control II
G05 P10000
Spline G05.1 Q2
(2) When the mirror image (G code/parameter/external signal) is canceled anywhere except at the mirror image center during the polar coordinate command mode, the absolute value and machine position will deviate. The mirror center is set with an absolute value and so if another mirror center is assigned in this state, the center may be set at an unforeseen position. Cancel the mirror image above the mirror center or, after cancellation, assign a positioning command using absolute value command that the radius and angle of the polar coordinate command are designated.
6. Interpolation Functions 6.13 Spiral/Conical Interpolation
90
6.13 Spiral/Conical Interpolation; G02.0/G03.1(Type1), G02/G03(Type2)
Function and purpose
This function carries out interpolation that smoothly joins the start and end points in a spiral. This interpolation is carried out for arc commands in which the start point and end point are not on the same circumference. There are two types of command formats, and they can be switched with the parameters.
Command format
G17 G02.1/G03.1 X__ Y__ I__ J__ P__ F__ ; (Type 1: #1272 ex08/bit2=0) G17 G02/G03 X__ Y__ I__ J__ Q__/L__/K__ F__ ; (Type 2: #1272 ex08/bit2=1) G17 : Rotation plane G02.1/G03.1 (Type 1) : Arc rotation direction (Type 1) G02/G03 (Type 2) : Arc rotation direction (Type 2) X Y : End point coordinates (Conical Interpolation when the axis other
than rotation plane axes is included.) I J : Arc center P : Number of pitches (number of rotations) (Type 1) Q/L/K (Type 2) : Incremental/decremental amount of radius /Number of
pitches(Number of spirals)/ Increment/decrement amount of height (Type 2)
F : Feedrate (tool path direction speed) Circular interpolation operations are carried out at the f1 speed by the commands above. The path is toward the end point, following a spiral arc path centered at the position designated by distance i (X axis direction) and distance j (Y axis direction) in respect to the start point. (1) The arc plane is designated by G17, G18 and G19. (Common for type 1 and 2) G17 XY plane G18 ZX plane G19 YZ plane (2) The arc rotation direction is designated by G02.1(G02) or G03.1(G03). (Common for type 1
and 2) G02.1(G02) Clockwise (CW) G03.1(G03) Counterclockwise (CCW) (3) The end point coordinates are designated with XYZ. (Common for type 1 and 2)
(Decimal point command is possible. Use mm (or inch) as the unit). When designation of arc plane axes is omitted, the coordinates of the start point are inherited. If the axis other than arc plane axes is designated, conical interpolation is applied.
(4) The arc center is designated with IJK. (Common for type 1 and 2)
(Decimal point command is possible. Use mm (or inch) as the unit.) I : Incremental designation in the X axis direction from the start point J : Incremental designation in the Y axis direction from the start point K : Incremental designation in the Z axis direction from the start point When either 1 axis of arc plane is omitted, the coordinates of the start point are inherited.
6. Interpolation Functions 6.13 Spiral/Conical Interpolation
91
(5) P designates the number of pitches (number of spirals). (Type 1)
The number of pitches and rotations is as shown below. Number of pitches
(0 to 99) Number of rotations
P0 Less than 1 rotation (Can be omitted.)
P1 1 or more rotation, less than 2 rotations
Pn n or more rotation, less than (n+1) rotations
(6) Q designates the increment/decrement amount of radius per spiral rotation. (Type 2)
The number of spiral rotations when the radius increment/decrement amount is specified can be calculated with the following expression. Number of rotations= | (arc end point radius — arc start point radius)) | / | increment/decrement amount of radius |
(7) L designates the number of pitches (number of spirals). (Type 2) (range: 0 to 99)
When omitted, L1 is designated. The number of pitches and rotations is as shown below.
Number of pitches (0 to 99) Number of rotations
L1 Less than 1 rotation L2 1 or more rotation,
less than 2 rotations Ln (n-1) or more rotations,
less than n rotations Q takes precedence over L if both Q and L have been designated at the same time. (8) K designates the increment/decrement amount of height per spiral rotation in conical
interpolation. (Type 2) The increment/decrement amount of height is designated with I/J/K for the axis other than arc plane. The relation between increment/decrement amount of height and the rotation plane is as shown below.
Rotation plane Increment/decrement amount of height
G18 J command G19 I command Other than G18/G19 K command
The number of rotations when the designation of increment/decrement amount of height is specified can be calculated with the following expression. Number of rotations = Height / | Increment/decrement amount of height | If Q, K and L have been designated at the same time, the order of precedence is Q>K>L. Decimal point command is possible in the range of the increment/decrement amount of radius and height. Use mm (or inch) as the unit.
6. Interpolation Functions 6.13 Spiral/Conical Interpolation
92
(9) In the following cases, a program error will occur.
(a) Items common for type 1 and 2
Settings Command range (Unit) Error
End point coordinate
Range of coordinate command (mm/inch) (Decimal point command is possible.)
If a value exceeding the command range is issued, program error (P35) will occur.
If an axis other than one which can be controlled with the command system is commanded, a program error (P33) will occur.
Arc center Range of coordinate command (mm/inch) (Decimal point command is possible.)
If a value exceeding the command range is issued, a program error (P35) will occur.
If an axis other than one which can be controlled with the command system is commanded, a program error (P33) will occur.
If rotation plane axis is not designated completely, a program error (P33) will occur.
Number of pitches
0 to 99 If a value exceeding the command range is issued, a program error (P35) will occur.
Feedrate Range of speed command (mm/min,inch/mi n) (Decimal point command is possible.)
If a value exceeding the command range is issued, a program error (P35) will occur.
(b) Items for type 2 only
Settings Command range (Unit) Error
Increment/ decrement amount of radius
Range of coordinate command (mm/inch) (Decimal point command is possible.)
If the sign of designated increment/decrement amount is opposite from that of the difference between the start point radius and the end point radius, a program error (P33) will occur.
If the end point position obtained from the speed and increment/decrement amount is larger than «SpiralEndErr (#8075)», a program error (P70) will occur.
Increment/ decrement amount of height
Range of coordinate command (mm/inch) (Decimal point command is possible.)
If the sign of designated increment/decrement amount is opposite from that of the movement direction of height, a program error (P33) will occur.
If the end point position obtained from the speed and increment/decrement amount is larger than «SpiralEndErr (#8075)», a program error (P70) will occur.
G02.1/0G3.1 Program error (P34) will occur if G02.1/G03.1 are used during type 2.
6. Interpolation Functions 6.13 Spiral/Conical Interpolation
93
Detailed description
(1) The arc rotation direction G02.1 is the same as G02, and G03.1 is the same as G03. (2) There are no R-designated arcs in spiral interpolation. (3) Conical cutting, tapered thread-cutting and other such machining operations can be
conducted by changing the start point and end point radius and commanding the linear axis simultaneously.
(4) Normally the spiral interpolation is automatically enabled with the arc commands (G02, G03) when the difference between the start point radius and the end point radius is less than the parameter setting value.
(5) The axis combination that can be simultaneously commanded depends on the specifications. The combination within that range is random.
(6) The feedrate is the constant tangential speed. (7) Simultaneous control by combining with tool radius compensation (G41, G42) is not possible. (8) The arc plane always follows G17, G18 and G19. The plane arc control is carried out by G17,
G18 and G19, even if designated by two addresses that do not match the plane. (9) Conical interpolation
When an axis designation other than the spiral interpolation plane is simultaneously designated, other axes are also interpolated in synchronization with the spiral interpolation.
6. Interpolation Functions 6.13 Spiral/Conical Interpolation
94
Example of program
(Example 1)
G91 G17 G01 X60. F500 ; Y140. ; G02.1 X60. Y0 I100. P1 F300 ; G01 X120 ; G90 G17 G01 X60. F500 ; Y140. ; G02.1 X120. Y140. I100. P1 F300 ; G01 X0 ;
Start point
End point
140.
60. 120. 160.
Y
W X
X60.
I100.
Center
(Example 2)
G91 G17 G01 X60. F500 ; Y140. ; G02.1 X60.0 Z100.0 I100. P1 F300 ; G01 X120 ;
Because this is the G17 plane, arc control is not carried out by X-Z.
Arc control is carried out by X-Y. (Example 3) In this example, the interpolation is truncated cone interpolation.
G17 G91 G02.1 X100. Z150. I150. P3 F500 ;
XY plane
XZ plane
X
X
X
Z Z
Y
W
W
Relation with other functions
(1) Items common for type 1 and 2
The start point and end point are not on the same arc, so normal line control is not applied correctly.
If there is no center command when geometric is valid, a program error (P33) will occur. (2) Items for type 2 only
If the spiral interpolation command is issued during the mirror image, a program error (P34) will occur.
If the spiral interpolation command is issued during the scaling, a program error (P34) will occur.
If the spiral interpolation command is issued during the corner chamfering/corner rounding command, a program error (P33) will occur.
6. Interpolation Functions 6.14 3-dimensional Circular Interpolation; G02.4, G03.4
95
6.14 3-dimensional Circular Interpolation; G02.4, G03.4
Function and purpose
To issue a circular command over a 3-dimensional space, an arbitrary point (intermediate point) must be designated on the arc in addition to the start point (current position) and end point. By using the 3-dimensional circular interpolation command, an arc shape determined by the three points (start point, intermediate point, end point) designated on the 3-dimensional space can be machined. An option is required to validate this function. If the option is not provided and the 3-dimensional circular interpolation command is issued, a program error (P39) will occur. 3-dimensional circular interpolation command
Start point (Current position)
End point
Intermediate point Z
X
Y
6. Interpolation Functions 6.14 3-dimensional Circular Interpolation; G02.4, G03.4
96
Command format
G02.4(G03.4) Xx1 Yy1 Zz1 1 ; Intermediate point designation (1st block)
Xx2 Yy2 Zz2 2 ; End point designation (2nd block) G02.4(G03.4) x1, y1, z1 x2, y2, z2
: 3-dimensional circular interpolation command (Cannot designate the rotation direction) : Intermediate point coordinates : End point coordinates : Arbitrary axis other than axis used as the reference in 3-dimensional circular interpolation (May be omitted)
The G02.4 and G03.4. operations are the same. (The rotation direction cannot be designated.) The axes used as the reference in 3-dimensional circular interpolation are the three basic axes
set with the parameters. The X, Y, Z address in the block may be omitted. The intermediate point coordinates omitted in
the 1st block become the start point coordinates, and the end point coordinates omitted in the 2nd block become the intermediate point coordinates.
When using the 3-dimensional circular interpolation command, an arbitrary axis can be commanded in addition to the orthogonal coordinate system (X, Y, Z) used as the reference. The arbitrary axis designated in the intermediate point designating block (1st block) will interpolate to the command point when moving from the start point to intermediate point. The arbitrary axis designated in the end point command block (2nd block) will interpolate to the command point when moving from the intermediate point to the end point. The number of arbitrary axes that can be commanded differs according to the number of simultaneous contour control axes. The total of the basic three axes used as the reference of the 3-dimensional circular interpolation and the arbitrary axes commanded simultaneously must be less than the number of simultaneous contour control axes.
6. Interpolation Functions 6.14 3-dimensional Circular Interpolation; G02.4, G03.4
97
Designating intermediate point and end point
When using the 3-dimensional circular interpolation command, an arc that exists over the 3-dimensional space can be determined by designating the intermediate point and end point in addition to the start point (current position). (Refer to following figure) So according to the command format, it is necessary to designate an intermediate point in the 1st block and an end point in the 2nd block. If only one block is designated, a program error (P74) will occur. Liner interpolation is applied when the end point match the start point in the 3-dimensional circular interpolation command. (Refer to «When liner interpolation is applied») Thus, a true circle (360-degree rotation) cannot be designated in the 3-dimensional circular interpolation. In addition, designate that an intermediate point is located in the middle of a start point and an end point. If the intermediate point is near the start point or the end point, arc accuracy may fall.
Designation of arc in 3-dimensional space
Start point (Current position)
End point
Intermediate point Plane including start point, intermediate point and end point
Center
As shown in the above figure, when three points (start point, intermediate point, end point) are specified on 3-dimensional space, arc center coordinates can be obtained. An arc center cannot be obtained if only two points are specified, and a liner interpolation is applied. If the intermediate point is near the start point or the end point, an error may occur when calculating arc center.
6. Interpolation Functions 6.14 3-dimensional Circular Interpolation; G02.4, G03.4
98
When liner interpolation is applied
In the following case, liner interpolation but 3-dimensional circular interpolation is applied. (1) When the start point, intermediate point, and end point are on the same line (refer to the
following figure) (If the end point exists between the start point and intermediate point, axes move in the order of start point, intermediate point, and end point.)
(2) When two points match in start point, a intermediate point, end point (Liner interpolation is applied even if the end point matches the start point to command true circle. When the start point matches the end point, axes move in order of the start point, an intermediate point, and an end point.)
When liner interpolation is applied
Start point (Current position)
Intermediate point (Block1)
End point (Block2)
When the three points are on the same line, liner interpolation is applied.
Start point (Current position)
End point (Block2)
Intermediate point (Block1)
Even if the end point exists between the start point and intermediate point, move in the order of start point, intermediate point, and end point.
Modal command
The 3-dimensional circular interpolation command G02.4 (G03.4) is a modal command belonging to 01 group. The command will remain valid until the other G command in the 01 group is issued. When the 3-dimensional circular interpolation command is carried out continuously, the end point of present command is the start point of next command.
Precautions
(1) If single block is valid and this command is operated, a block stop is carried out at an
intermediate point and the end point. (2) The speed command during 3-dimensional circular interpolation is the tangential speed on
arc. (3) When 3-dimensional circular interpolation is commanded while incremental command is valid,
the relative position of the intermediate point in respect to the start point is designated in the intermediate point designation block, and the relative position of the end point in respect to the intermediate point is designated in the intermediate point designation block.
(4) The path of 3-dimentional circular interpolation during graphic check is drawn as linear at each range from start point to intermediate point and from intermediate point to end point.
6. Interpolation Functions 6.14 3-dimensional Circular Interpolation; G02.4, G03.4
99
Relation with other functions
(1) Commands that cannot be used
(a) G code command which leads to a program error during 3-dimensional circular interpolation modal
G code Function name Program error G05 Pn High-speed machining mode P34 G05 P10000 High-speed high-accuracy control II P34 G05.1 Q0/G05.1 Q1 High-speed high-accuracy control I P34 G07.1 Cylindrical interpolation P485 G12/G13 Circular cutting CW/CCW P75 G12.1 Polar coordinate interpolation P485 G16 Polar coordinate command P75 G41/G42 Tool radius compensation P75 G41/G42 3-dimentional tool radius compensation P75 G41.1/G42.1 Normal line control P75 G43/G44 Tool length compensation P75 G51 Scaling P75 G51.1 Mirror image P75 G66/G66.1 User macro P75 G67 User macro P276 G68 Programmable coordinate rotation P75 G68 3-dimensional coordinate conversion P921 G73/G74/G76/G81/G82/G83 / G84/G85/G86/G87/G88/G89
Fixed cycle P75
(b) G code command which leads to a program error when 3-dimensional circular interpolation
is commanded G code modal Function name Program error
G05 Pn High-speed machining mode P34 G05 P10000 High-speed high-accuracy control II P34 G05.1 Q1 High-speed high-accuracy control I P34 G07.1 Cylindrical interpolation P481 G12.1 Polar coordinate interpolation P481 G16 Polar coordinate command P75 G41/G42 Tool radius compensation P75 G41/G42 3-dimentional tool radius compensation P75 G41.1/G42.1 Normal line control P75 G43/G44 Tool length compensation P75 G51 Scaling P75 G51.1 Mirror image P75 G66/G66.1 User macro P75 G68 Programmable coordinate rotation P75 G68 3-dimensional coordinate conversion P922
(2) Functions that cannot be used If following functions are used in 3-dimensional circular interpolation, alarm will occur.
Chopping Mirror image by parameter setting Macro interruption Mirror image by external input Corner chamfering / corner R
Restrictions may be added for other functions. Refer to explanation of each function.
6. Interpolation Functions 6.15 NURBS Interpolation
100
6.15 NURBS Interpolation
Function and purpose
This function realizes NURBS (Non-Uniform Rational B-Spline) curve machining by simply commanding NURBS curve parameters (stage, weight, knot, control point), which is used for the curved surface/line machining, without replacing the path with minute line segments. This function operates only in the high-speed high-accuracy control II mode, so the high-speed high-accuracy control II option is required. During NURBS interpolation, interpolation takes place at the commanded speed. However, if the curvature is large, the speed is clamped so that the machine’s tolerable acceleration rate is not exceeded.
Command format
G05 P10000 ; G06.2 Pp Kk1 Xx1 Yy1 Zz1 Rr1 Ff;
High-speed high-accuracy control II mode ON NURBS interpolation ON
Kk2 Xx2 Yy2 Zz2 Rr2; Kk3 Xx3 Yy3 Zz3 Rr3; Kk4 Xx4 Yy4 Zz4 Rr4; — — — — — — — — — — — — — — — — — — — — Kkn Xxn Yyn Zzn Rrn; Kkn+1; Kkn+2; Kkn+3;
Kkn+4; NURBS interpolation OFF
G05 P0; High-speed high-accuracy control II mode OFF
G05 P10000 G06.2 Qq Pp
: High-speed high-accuracy control II mode : NURBS interpolation : Set the stage of the NURBS curve. Designate in the same block as G06.2 command. The NURBS curve of the stage p will be (p-1)th curve. When omitted, Pp means the same as P4. (Example) P2: Primary curve (liner)
Kkn : Knot Set the knot for each NURBS interpolation block. Set the same value for the knot in the 1st block to the stage p block. NURBS interpolation is terminated if there is a block exclusively with knot.
Xxn Yyn Zzn : Control point coordinate value Designate the same coordinate value for the 1st block control point as that designated right before NURBS interpolation.
Rrn : Control point weight Set the weight of each NURBS interpolation control point.
Ff : Interpolation speed (May be omitted)
6. Interpolation Functions 6.15 NURBS Interpolation
101
Detailed description
(1) Designate the stage P for the 1st block of NURBS interpolation. (2) Designate the same coordinate value for the 1st block control point of NURBS interpolation as
that designated right before NURBS interpolation. (3) Designate all axes to be used in the subsequent NURBS interpolation blocks for 1st block of
NURBS interpolation (4) Set the same value for knot K from the 1st block of NURBS interpolation to setting value block
of the stage P. (5) Command knot K exclusive block of the same number as the setting value of the stage P for
terminating NURBS interpolation. At this time, set the same value for knot K setting.
(x3,y3,z3) (x4,y4,z4)
(xn,yn,zn)
Passes through control point
NURBS interpolation curve
(x1,y1,z1)
(x2,y2,z2)
(Note) If an exclusive knot is commanded after NURBS interpolation immediately, NURBS
interpolation mode is active again. An exclusive knot that is commanded after NURBS interpolation immediately is the same meaning as following command. G06.2 Pp Km Xxn Yyn Zzn R1.0
6. Interpolation Functions 6.15 NURBS Interpolation
102
Example of program
The example of program that has 4 stages (cubic curve) and 11 control points is shown below.
Control point P0 P1 P2 P3 P4 P5 P6 P7 P8 P9 P10
Knot 0.0 0.0 0.0 0.0 1.0 2.0 3.0 4.0 5.0 6.0 7.0 8.0 8.0 8.0 8.0
: : G05 P10000; G90 G01 X0. Y0. Z0. F300; G06.2 P4 X0. Y0. R1. K0; P0 X1.0 Y2.0 R1. K0; P1 X2.5 Y3.5 R1. K0; P2 X4.4 Y4.0 R1. K0; P3 X6.0 Y0.5 R1. K1; P4 X8.0 Y0.0 R1. K2; P5 X9.5 Y0.5 R1. K3; P6 X11.0 Y2.0 R1. K4; P7 X10.5 Y4.5 R1. K5; P8 X8.0 Y6.5 R1. K6; P9 X9.5 Y8.0 R1. K7; P10 K8; K8; K8; K8; G05 P0; : :
0
1
2
3
4
5
6
7
8
9
0 2 4 6 8 10 12 P0(0.0,0.0)
P1(1.0,2.0)
P2(2.5,3.5) P3(4.4,4.0)
P4(6.0,0.5) P5(8.0,0.0)
P6(9.5,0.5)
P9(8.0,6.5)
P10(9.5,8.0)
X
Y
P7(11.0,2.0)
P8(10.5,4.5)
Passes through control point
NURBS interpolation curve
6. Interpolation Functions 6.15 NURBS Interpolation
103
Relation with other functions
(1) G code/Feed/Miscellaneous functions
All the G code, feedrate and MSTB code cannot be set during NURBS interpolation. However, when the fixed cycle G code is commanded in the same block where G06.2 is commanded, the fixed cycle G code is ignored. If a command other than the axis address designated in the 1st block of NURBS interpolation, R and K is commanded, a program error will occur.
(2) Data format
(a) Optional block skip «/» Cannot be set in the NURBS interpolation 2nd block or after.
(b) Control IN «(«and Control OUT «)» Cannot be set in the NURBS interpolation 2nd block or after.
(c) Local variables and common variables Can be referred but cannot be set in the NURBS interpolation. Setting the variables causes a program error (P29).
(d) System variables Cannot be referred nor set in the NURBS interpolation; a program error (P29) will occur.
(3) Interruption/restart
The validity of program interruption/restart is shown below.
Type During NURBS interpolation
Single block Valid (Note 1) Feed hold Valid Reset Valid (Note 2) Program stop Invalid Optional stop Invalid Manual interruption Invalid (Note 3) MDI interruption Invalid Restart search Invalid Macro interruption Invalid (Note 4) PLC interruption Invalid (Note 5)
(Note 1) A single block stop is carried out at only the last control points. The single block stop is not applied during NURBS interpolation.
(Note 2) NURBS interpolation mode is canceled with Reset (Reset1/Reset2/Reset&Rewind). (Note 3) The operation differs according to the manual absolute signal status. When the manual absolute signal OFF
NURBS interpolation is carried out in the state where axis-coordinate system is shifted by the manual absolute movement amount.
When the manual absolute signal ON At automatic start after manual interruption, a program error (P554) will occur after moving the by the remaining distance. Note that the operation can run continually if returning the axis to the original position after manual interruption.
(Note 4) «Macro interrupt» signal (UIT) is ignored. (Note 5) «PLC interrupt» signal (PIT) is ignored.
(4) Graphic check NURBS interpolation cannot be applied during graphic check (continuous/step check). Linear interpolation that connects the control points is applied during graphic check.
6. Interpolation Functions 6.15 NURBS Interpolation
104
Precautions
(1) Target axes for NURBS interpolation are 3 basic axes. (2) Command the control point for all the axes for which NURBS interpolation is carried out in the
1st block (G06.2 block). A program error (P32) will occur if an axis which was not commanded in the 1st block is commanded in the 2nd block or after.
(3) The first control point (G06.2 block coordinate value) should be commanded as the start point
of the NURBS curve. Thus, command so that it matches the end point of the previous block. A program error will occur if the points do not match.
(4) The command range of the weight is 0.0001 to 99.9999. Even if the decimal point is omitted,
the value will be handled as the one with a decimal point. If «1» is commanded, the result will be the same as «1.0». If more than 5 digits are commanded
after the decimal point, a program error (P33) will occur. (5) The knot command cannot be omitted, and must be commanded in each block. A program
error (P33) will occur if omitted. (6) As with knot, in the same manner as weight, up to 4 digits can be commanded after the
decimal point. Even if the decimal point is omitted, the value will be handled as the one with a decimal point.
If «1» is commanded, the result will be the same as «1.0». If more than 5 digits are commanded after the decimal point, a program error (P33) will occur.
(7) As with knot, command the same or greater value than the previous block. If a smaller value
than previous block is set, a program error (P551) will occur. (8) NURBS interpolation cannot be applied during graphic check (continuous/step check). Linear interpolation that connects the control points is applied during graphic check. (9) NURBS interpolation mode is canceled with Reset(Reset1/Reset2/Reset&Rewind). (10) NURBS interpolation can be commanded in only the following modes. If NURBS interpolation
is commanded in other than the following modes, the program error (P29) will occur.
Type Mode in which NURBS interpolation can be commanded
G group 5 Asynchronous feed (G94) G group 7 Tool radius compensation cancel (G40) G group 8 Tool length compensation +/-(G43/G44)
Tool length compensation cancel (G49) G group 9 Fixed cycle cancel (G80) G group 11 Scaling cancel (G50) G group 13 High-accuracy control 1 ON (G61.1)
Cutting mode (G64) G group 14 User macro modal call cancel (G67) G group 15 Normal line control cancel (G40.1) G group 16 Programmable coordinate rotation mode OFF
/3-dimensional coordinate conversion mode OFF (G69)
G group 17 Constant surface speed control OFF (G97) G group 18 Polar coordinate command OFF (G15) G group 19 G command mirror image cancel (G50.1) G group 21 Polar coordinate interpolation cancel (G13.1)
— Not during the parameter coordinate rotation — Not during the mirror image by parameter setting — Not during the mirror image by external input
6. Interpolation Functions 6.16 Hypothetical Axis Interpolation; G07
105
6.16 Hypothetical Axis Interpolation; G07
Function and purpose
Take one of the axes of the helical interpolation or spiral interpolation, including a linear axis, as a hypothetical axis (axis with no actual movement) and perform pulse distribution. With this procedure, an interpolation equivalent to the helical interpolation or spiral interpolation looked from the side (hypothetical axis), or SIN or COS interpolation, will be possible. Normal helical interpolation
0.
5.
10.
-5.
-10.
20. 40. -10.0.
X axis
Y axisZ axis
X axis
Helical interpolation in the hypothetical axis interpolation mode
0.
5.
10.
-5.
-10.
20. 40. -10.0.
X axis Hypothetical axis
(Y axis in this example) does not move actually.
X axis
Y axisZ axis
To perform the SIN interpolation on Z-X plane, execute the helical interpolation (Y-X plane: G17 G02) with Y axis which is designated as the hypothetical axis.
Command format
G07 0 ; Hypothetical axis interpolation mode ON
G07 1 ; Hypothetical axis interpolation mode cancel
: Designate the axis for which hypothetical axis interpolation is performed.
6. Interpolation Functions 6.16 Hypothetical Axis Interpolation; G07
106
Detailed description
(1) During G070 to G071, axis will be the hypothetical axis. (2) Any axis among the NC axes can be designated as the hypothetical axis. (3) Multiple axes can be designated as the hypothetical axis. (4) The number other than 0 (hypothetical axis interpolation mode ON) or 1 (cancel) is
commanded, it will be handled as 1 (cancel). However, when only the axis name is designated with no number, it will be handled as 0 (mode ON).
Example of program
N01 G07 Y0 ; Y axis is handled as hypothetical axis. N02 G17 G02 X0. Y0. Z40. I0. J-10. P2 F50; SIN interpolation is executed on X-Z plane. N03 G07 Y1 ; Y axis is returned to the actual axis.
0.
5.
10.
-5.
-10.
20. 40.
X axis
Z axis
Precautions
(1) Interpolation functions that are used for hypothetical axis interpolation are helical interpolation
and spiral interpolation. (2) Cancel the hypothetical axis interpolation before the high-speed high-accuracy control 2
(G05P10000) is commanded. (3) The hypothetical axis interpolation is valid only in the automatic operation. It is invalid in the
manual operation mode. Handle interruption is valid even for the hypothetical axis, that is, axis will move by the interrupted amount.
(4) Movement command for the hypothetical axis will be ignored. The feedrate will be distributed in the same manner as actual axis.
(5) The protection functions such as interlock or stored stroke limit are valid for the hypothetical axis.
(6) Even when the hypothetical axis is applied for the hypothetical axis again, no error will occur and the hypothetical mode will be continued.
(7) When the hypothetical axis cancel is commanded to the actual axis, no error will occur and the axis is actual as it is.
(8) The hypothetical axis will be canceled by carrying out the reset 2 or reset & rewind.
7. Feed Functions 7.1 Rapid Traverse Rate
107
7. Feed Functions 7.1 Rapid Traverse Rate
Function and purpose
The rapid traverse rate can be set independently with parameters for each axis. The available speed ranges are from 1 mm/min to 10000000 mm/min. The upper limit is subject to the restrictions imposed by the machine specifications. Refer to the specifications manual of the machine for the rapid traverse rate settings. The feedrate is valid for the G00, G27, G28, G29, G30 and G60 commands. Two paths are available for positioning: the interpolation type where the area from the start point to the end point is linearly interpolated or the non-interpolation type where movement proceeds at the maximum speed of each axis. The type is selected with parameter «#1086 G0Intp». The positioning time is the same for each type. If the high-accuracy control mode’s rapid traverse rate is set, the axis will move at that feed rate during high-accuracy control, high-speed high-accuracy control I/II, high-accuracy spline control or SSS control. If the value set for the high-accuracy control mode rapid traverse rate is 0, the axis will move at
the rapid traverse rate. The high-accuracy control mode rapid traverse rate can be set independently for each axis. The high-accuracy control mode rapid traverse rate is effective for the G00, G27, G28, G29, G30
and G60 commands. Override can be applied on the high-accuracy control mode rapid traverse rate using the external
signal supplied.
7.2 Cutting Feedrate
Function and purpose
The cutting feedrate is assigned with address F and 8 digits (F8-digit direct designation). The F8 digits are assigned with a decimal point for a 5-digit integer and a 3-digit fraction. The cutting feedrate is valid for the G01, G02, G03, G02.1 and G03.1 commands. If the high-accuracy control mode’s cutting clamp speed is set, the cutting feed rate will be clamped at that feedrate during high-accuracy control, high-speed high-accuracy control, high-accuracy spline control or SSS control. If the value set for the high-accuracy control mode cutting clamp speed is 0, the axis will be
clamped at the cutting feed clamp speed. The cutting feedrate is clamped with high-accuracy control mode cutting clamp speed in the
parameter. (Example)
Feedrate G1 X100. Y100. F200 ; G1 X100. Y100. F123.4 ; G1 X100. Y100. F56.789 ;
200.0mm/min 123.4mm/min 56.789mm/min
F200 or F200.000 gives the same rate.
Speed range that can be commanded (when input setting unit is 1m)
Command mode Feed rate command range Remarks
mm/min 0.001 to 10000000 mm/min
inch/min 0.0001 to 1000000 inch/min
/min 0.001 to 10000000 /min
(Note 1) A program error (P62) results when there is no F command in the first cutting command (G01, G02, G03) after the power has been switched on.
7. Feed Functions 7.3 F1-digit Feed
108
7.3 F1-digit Feed
Function and purpose
By setting the F1-digit feed parameter, the feedrate which has been set to correspond to the 1-digit number following the F address serves as the command value. When F0 is assigned, the rapid traverse rate is established and the speed is the same as for G00. (G modal does not change, but the acceleration/deceleration method is followed by the settings for the rapid traverse.) When F1 to F5 is assigned, the feedrate set to correspond to the command serves as the command value. The command greater than F6 is considered to be the normal cutting feedrate. The F1-digit command is valid in a G01, G02, G03, G02.1 or G03.1 modal. The F1-digit command can also be used for fixed cycle.
Detailed description
The override function of the feedrate which is set in accordance to the F1-digit is performed by using the 1st manual handle. (Feedrate cannot be changed with the 2nd or 3rd handle.) The amount by which the feedrate can be increased or reduced is determined by the following formula.
F = FM
K (number of manual handle pulse generator pulses)
Where «+» means increase, and «-» means reduction. K : Operation constant (This is the number of FM divisions, and is the calculated constant of
the increment/decrement speed per scale of the manual handle pulse generator.) This is set with the base specification parameter «#1507 F1_K».
FM : This is the clamp speed of F1 to F5 This is set with the base specification parameter «#1506 F1_FM».
Set the corresponding speed of F1 to F5 with the base specification parameters «#1185 spd_F1» to «#1189 spd_F5» respectively. The increase/reduction range is from «0» to the set value of the parameter «#1506 F1_FM». Operation alarm (104) will occur when the feedrate is 0. (1) Operation method
(a) Make the F1-digit command valid. (Set the base specification parameter «#1079 F1digt» to 1.)
(b) Set FM and K. Setting range K : 1 to 32767 (Base specification parameter «#1507 F1_K») FM : 0 to Fmax (mm/min) (Base specification parameter «#1506 F1_FM»)
(c) Set F1 to F5. (Base specification parameter «1185 spd_F1» to «#1189 spd_F5»)
(2) Special notes (a) Use of both the F1-digit command and normal cutting feedrate command is possible when
the F1-digit is valid. (Example 1)
F0 Rapid traverse rate F1 to F5 F1-digit F6 or more Normal cutting feedrate command
(b) F1 to F5 are invalid in the G00 mode and the rapid traverse rate is established instead.
(c) If F0 is used in the G02 or G03 mode, a program error (P121) will result.
7. Feed Functions 7.3 F1-digit Feed
109
(d) When F1. to F5. (with decimal point) are assigned, the 1mm/min to 5mm/min direct commands are established instead of the F1-digit command.
(e) When the commands are used with the millimeter or degree units, the feedrate set to correspond to F1 to F5 serves as the assigned speed mm ()/min.
(f) When the commands are used with inch units, one-tenth of the feedrate set correspond to F1 to F5 serves at the assigned speed inch/min.
(g) The number of manual handle pulses is 1 pulse per scale unit regardless of the scaling factor.
(h) During a F1-digit command, the F1-digit number and F1-digit command signal are output as the PLC signals.
(i) Even if the F1-digit feed commanded during the feed per rotation (G95) is considered as a regular F command (direct value command).
(3) F1-digit and G commands (a) 01 group G command in same block as F1-digit commands
Executed feedrate Modal display rate G modal G0F0 F0G0 Rapid traverse rate 0 G0
G0F1 F1G0 Rapid traverse rate 1 G0
G1F0 F0G1 Rapid traverse rate 0 G1
G1F1 F1G1 F1 contents 1 G1
(b) F1-digit and unmodal commands may be assigned in the same block. In this case, the unmodal command is executed and at the same time the F1-digit modal command is updated.
(4) Example of arithmetic constant K setting
When the handle scale unit is to be made 10mm/min. FM is made 15000 mm/min:
F = 10 = 15000 K
Therefore, K is 1500. The feed rate is made F (1 to 5) 10 (mm/min) by rotating the handle through one scale unit.
(5) Valid manual handle conditions The manual handle is valid during cutting feed (F1 to F5), automatic start, F1-digit valid and manual handle valid switch ON at the machine side as well as in the MDI mode, tape mode or memory mode provided that the machine lock (machine lock rapid traverse) or dry run status has not been established. The function cannot be used when the handle specifications have not been provided.
7. Feed Functions 7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed)
110
7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed); G94, G95
Function and purpose
Using the G95 command, it is possible to assign the feed amount per rotation with an F code. When this command is used, the rotary encoder must be attached to the spindle. When the G94 command is issued the per-minute feed rate will return to the designated per-minute feed (asynchronous feed) mode.
Command format
G94; G95;
G94 : Per-minute feed (mm/min) (asynchronous feed) G95 : Per-revolution feed (mm/rev) (synchronous feed)
The G95 command is a modal command and so it is valid until the G94 command (per-minute feed) or G93 command (inverse time feed) is next assigned.
(1) The F code command range is as follows.
The movement amount per spindle revolution with synchronous feed (per-revolution feed) is assigned by the F code and the command range is as shown in the table below. Metric input
Input command unit
system B (0.001mm) C (0.0001mm)
Command mode Feed per minute Feed per rotation Feed per minute Feed per rotation
Command address F (mm/min) E (mm/rev) F (mm/min) E (mm/rev)
Minimum command unit
1 (= 1.000), (1. = 1.000)
1 (= 0.001), (1. = 1.000)
1 (= 1.0000), (1. = 1.0000)
1 (= 0.0001), (1. = 1.0000)
Command range
0.001 ~1000000.000
0.001 ~999.999
0.0001 ~1000000.0000
0.0001 ~999.9999
Input
command unit system
D (0.00001mm) E (0.000001mm)
Command mode Feed per minute Feed per rotation Feed per minute Feed per rotation
Command address F (mm/min) E (mm/rev) F (mm/min) E (mm/rev)
Minimum command unit
1 (= 1.00000), (1. = 1.00000)
1 (= 0.00001), (1. = 1.00000)
1 (= 1.000000), (1. = 1.000000)
1 (= 0.000001), (1. = 1.000000)
Command range
0.00001 ~1000000.00000
0.00001 ~999.99999
0.000001 ~1000000.000000
0.000001 ~999.999999
7. Feed Functions 7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed)
111
Inch input
Input command unit
system B (0.0001inch) C (0.00001inch)
Command mode Feed per minute Feed per rotation Feed per minute Feed per rotation
Command address F (inch/min) E (inch/rev) F (inch/min) E (inch/rev)
Minimum command unit
1 (= 1.0000), (1. = 1.0000)
1 (= 0.0001), (1. = 1.0000)
1 (= 1.00000), (1. = 1.00000)
1 (= 0.00001), (1. = 1.00000)
Command range
0.0001 ~ 100000.0000
0.0001 ~ 999.9999
0.00001 ~ 100000.00000
0.00001 ~ 999.99999
Input
command unit system
D (0.000001inch) E (0.0000001inch)
Command mode Feed per minute Feed per rotation Feed per minute Feed per rotation
Command address F (inch/min) E (inch/rev) F (inch/min) E (inch/rev)
Minimum command unit
1 (= 1.000000), (1. = 1.000000)
1 (= 0.000001), (1. = 1.000000)
1 (= 1.0000000), (1. = 1.0000000)
1 (= 0.0000001), (1. = 1.0000000)
Command range
0.000001 ~100000.000000
0.000001 ~999.999999
0.0000001 ~100000.0000000
0.0000001 ~999.9999999
(2) The effective speed (actual movement speed of machine) under per-revolution feed conditions
is given in the following formula (Formula 1). FC = F N OVR ….. (Formula 1)
Where FC = Effective rate (mm/min, inch/min) F = Commanded feedrate (mm/rev, inch/rev) N = Spindle speed (r/min) OVR = Cutting feed override
When a multiple number of axes have been commanded at the same time, the effective rate FC in formula 1 applies in the vector direction of the command.
(Note 1) The effective rate (mm/min or inch/min), which is produced by converting the
commanded speed, the spindle speed and the cutting feed override into the per-minute speed, appears as the FC on the monitor 1. Screen of the setting and display unit.
(Note 2) When the above effective rate exceeds the cutting feed clamp rate, it is clamped at
that clamp rate. (Note 3) If the spindle speed is zero when synchronous feed is executed, operation alarm
«105» results. (Note 4) Under dry run conditions, asynchronous speed applies and the axes move at the
manual feed rate (mm/min, inch/min, /min). (Note 5) The fixed cycle G84 (tapping cycle) and G74 (reverse tapping cycle) are executed to
the feed mode that is already designated. (Note 6) Whether asynchronous feed (G94) or synchronous feed (G95) is applied when the
power is switched on or when M02 or M30 is executed is set with the parameter «#1074 I_Sync».
7. Feed Functions 7.5 Inverse Time Feed; G93
112
7.5 Inverse Time Feed; G93
Function and purpose
During inside cutting when machining curved shapes with radius compensation applied, the machining speed on the cutting surface becomes faster than the tool center feedrate. Therefore, problems such as reduced accuracy may occur. This reduced accuracy can be prevented with inverse time feed. This function can, in place of normal feed commands, issue one block of machining time (inverse) in F commands. The machining speed on the cutting surface is constantly controlled, even if radius compensation is applied to the machining program that expresses the free curve surface with fine segment lines. Note that when the calculated machining time exceeds the cutting feed clamp speed, the F command value in the inverse time feed follows the cutting feed clamp speed.
Regular F command
Actual machining speed
Large Small
F command
The speed of tool center is commanded, thus the actual speed at the cutting surface may become larger or smaller.
Inverse time feed
Same
F command
The actual speed at the cutting surface is commanded, thus, the speed will be constant and machining speed can be kept as that was commanded regardless of the tool radius.
Command format
G93 ; Inverse time feed
Inverse time feed (G93) is a modal command. Once commanded, it is valid until feed per minute or feed per revolution is commanded.
G00 Xx1 Yy1 ; G93; Inverse time feed mode ON G01 Xx2 Yy2 Ff2; In inverse time feed mode G02 Xx3 Yy3 Ii3 Jj3 Ff3; : G94(G95); Inverse time feed mode OFF
In movement blocks, since processing time is commanded to a line segment, command the feedrate «F» each time.
7. Feed Functions 7.5 Inverse Time Feed; G93
113
Detailed description
(1) Inverse time feed (G93) is a modal command. Once commanded, it is valid until feed per
minute (G94) or feed per revolution (G95) is commanded, or until a reset (M02, M30, etc.) is executed.
(2) Command method of F command values in inverse time feed
Metric command (G21) Inch command (G20)
During linear mode (G01)
Cutting point feedrate (mm/min) Line segment length (mm)
Cutting point feedrate (inch/min) Line segment length (inch)
During arc mode (G02, G03) (G02.1, G03.1)
Cutting point feedrate (mm/min) Start point arc radius (mm)
Cutting point feedrate (inch/min) Start point arc radius (inch)
B 0.001 to 999999.999(1/min) C 0.0001 to 999999.9999(1/min) D 0.00001 to 999999.99999(1/min)
Command range
E 0.000001 to 999999.999999(1/min) (3) The initial modal after a restart is G94 (feed per minute) or G95 (feed per revolution). (4) The feedrate of the block inserted in tool radius compensation and corner R/C is the same
speed as the feedrate of the block immediately before it. (5) The feedrate of the block inserted in C axis normal line control (normal line control type II) is the
same speed as the feedrate of the movement block after turning.
Precautions
(1) The initial modal after a restart is G94 (feed per minute) or G95 (feed per revolution). (2) The F command in G93 modal is unmodal. Issue an F command for each block. The program
error (P62) will occur in blocks with no F command. (3) The program error (P62) will occur when F0 is commanded. (4) An F command is necessary when changing from G93 to G94/G95. The program error
(P62) will occur if there is no F command. (5) The feed function is clamped at the maximum cutting speed. Consequently, the feed may be
slower than the commanded speed. (6) If an extremely slow speed such as F0.001 is designated, an error will occur in the machining
time.
7. Feed Functions 7.5 Inverse Time Feed; G93
114
Example of program
When using inverse time feed during tool radius compensation
N01 G90 G00 X80. Y-80. ;
N02 G01 G41 X80 Y-80. D11 F500 ;
N03 X180. ;
N04 G02 Y-280. R100. ;
N05 G03 Y-480. R100. ;
N06 G02 Y-680. R100. ;
N07 G01 X80. F500 ;
N08 Y-80. ;
N09 G04 X80. Y-80. ;
N10 M02 ;
Feed per minute
N01 G90 G00 X80. Y-80. ;
N02 G01 G41 X80. Y-80. D11 F500 ;
N03 X180. ;
N04 G93 G02 Y-280. R100. F5 ;
N05 G03 Y-480. R100. F5 ;
N06 G02 Y-680. R100. F5 ;
N07 G94 G01 X80. F500 ;
N08 Y-80. ;
N09 G04 X80. Y-80. ;
N10 M02 ;
Inverse time feed
(Fig. 3)
N4
N6
N5
Comparison between feed per minute and inverse time feed
(Assuming that tool radius is 10. [mm]) (Unit: mm/min) Feed per minute Inverse time feed Location
Sequence No.
Feedrate of tool center
Feedrate of cutting point
Feedrate of tool center
Feedrate of cutting point
N04 F500 F450 F550 F500 N05 F500 F550 F450 F500 N06 F500 F450 F550 F500
The block seam protrudes due to the cutting speed change at the block seam.
The feedrate follows the command regardless of the tool radius.
7. Feed Functions 7.5 Inverse Time Feed; G93
115
Relation with other functions
(1) Scaling (G51)
When using a scaling function, issue a F command for the shape after scaling. For example, if a double-size scaling is carried out, the machining distance will be twice. Thus, if executing a cutting at the same speed as that of before scaling, command the value (F) calculated by dividing F value by the multiples of scaling.
Feedrate (mm/min) F =
Distance (mm)
F F’=
2
Shape after scaling (Double size)
F
(2) High-speed machining mode II (G05P2)
With the inverse time feed (G93) modal, high-speed machining mode II (G05P2) is operated in the inverse time feed mode, instead of high-speed machining mode. High-speed machining mode will be valid when the inverse time feed mode is canceled.
(3) If the speed calculated in the G93 mode exceeds the speed range at the feed per minute, clamping is performed at the clamp speed set with parameters.
(4) The program error (P125) will occur when the commands below are issued in the inverse time feed (G93) mode.
G code Function G02.3, G03.3 Exponential interpolation G06.2 NURBS interpolation G12 Circular cutting CW G13 Circular cutting CCW G31~G31.3 Skip G33 Thread cutting G34~G36, G37 Special fixed cycle G37.1 Automatic tool length measurement G73~G89 Fixed cycle G96 Constant surface speed control ON
(5) The program error (P125) will occur if inverse time feed (G93) is commanded in the following
modes. G code Function
G02.3, G03.3 Exponential interpolation G33 Thread cutting G73~G89 Fixed cycle G96 Constant surface speed control ON
7. Feed Functions 7.6 Feedrate Designation and Effects on Control Axes
116
7.6 Feedrate Designation and Effects on Control Axes
Function and purpose
It has already been mentioned that a machine has a number of control axes. These control axes can be divided into linear axes which control linear movement and rotary axes which control rotary movement. The feedrate is designed to assign the displacement speed of these axes, and the effect exerted on the tool movement speed which poses problems during cutting differs according to when control is exercised over the linear axes or when it is exercised over the rotary axes. The displacement amount for each axis is assigned separately for each axis by a value corresponding to the respective axis. The feedrate is not assigned for each axis but assigned as a single value. Therefore, when two or more axes are to be controlled simultaneously, it is necessary to understand how this will work for each of the axes involved. The assignment of the feedrate is described with the following related items.
When controlling linear axes
Even when only one machine axis is to be controlled or there are two or more axes to be controlled simultaneously, the feed rate which is assigned by the F code functions as a linear speed in the tool advance direction. (Example) When the feedrate is designated as «f» and linear axes (X and Y) are to be controlled:
P (Tool start point)
P2 (Tool end point)
Speed in this direction is «f»
Y
Xx
y
Feedrate for X axis = f x x x2 + y2
Feedrate for Y axis = f x y x2 + y2
When only linear axes are to be controlled, it is sufficient to designate the cutting feed in the program. The feedrate for each axis is such that the designated rate is broken down into the components corresponding to the movement amounts.
7. Feed Functions 7.6 Feedrate Designation and Effects on Control Axes
117
(Example) When the feedrate is designated as «f» and the linear axes (X and Y) are to be controlled using the circular interpolation function:
The rate in the tool advance direction, or in other words the tangential direction, will be the feedrate designated in the program.
Linear speed is «f» y
x
Y
Xi
P2
P1
In this case, the feed rate of the X and Z axes will change along with the tool movement. However, the combined speed will always be maintained at the constant value «f».
When controlling rotary axes
When rotary axes are to be controlled, the designated feedrate functions as the rotary speed of the rotary axes or, in other words, as an angular speed. Consequently, the cutting feed in the tool advance direction, or in other words the linear speed, varies according to the distance between the center of rotation and the tool. This distance must be borne in mind when designating the feedrate in the program. (Example) When the feedrate is designated as «f» and rotary axis (CA) is to be controlled («f» units
= /min)
Rotation center
P2(tool end point)
P1 (tool start point)
Angular speed is «f»
Linear speed is : c
rf 180
r
In this case, in order to make the cutting feed (linear feed) in the tool advance direction «fc» :
fc = f r 180
Therefore, the feedrate to be designated in the program must be :
f = fc 180 r
7. Feed Functions 7.6 Feedrate Designation and Effects on Control Axes
118
When linear and rotary axes are to be controlled at the same time
The controller proceeds in exactly the same way whether linear or rotary axes are to be controlled. When a rotary axis is to be controlled, the numerical value assigned by the coordinate word (A, B, C) is the angle and the numerical values assigned by the feedrate (F) are all handled as linear speeds. In other words, 1 of the rotary axis is treated as being equivalent to 1mm of the linear axis. Consequently, when both linear and rotary axes are to be controlled simultaneously, the components for each axis of the numerical values assigned by F will be the same as previously described «When controlling linear axes». However, although in this case both the size and direction of the speed components based on linear axis control do not vary, the direction of the speed components based on rotary axis control will change along with the tool movement (their size will not change). This means, as a result, that the combined tool advance direction feedrate will vary along with the tool movement.
(Example) When the feed rate is designated as «f» and Linear (X) and rotary (C) axes are to be
controlled simultaneously. In the X-axis incremental command value is «x» and the C-axis incremental command values is «c»:
Rotation center
Size and direction are fixed for fx. Size is fixed for fc but direction varies. Both size and direction vary for ft.
P1
x
fc
c
fc ft
fx
fx
ft r
P2
7. Feed Functions 7.6 Feedrate Designation and Effects on Control Axes
119
X-axis feedrate (linear speed) «fx» and C-axis feedrate (angular speed) «» are expressed as:
fx = f x x2 + c2
……………………………………………………………………………. (1)
= f c x2 + c2
…………………………………………………………………………….. (2)
Linear speed «fc» based on C-axis control is expressed as:
fc = r 180 …………………………………………………………………………………….. (3)
If the speed in the tool advance direction at start point P1 is «ft» and the component speeds in the X-axis and Y-axis directions are «ftx» and «fty», respectively, then these can be expressed as:
ftx = -rsin ( 180 )
180 + fx ……………………………………………………… (4)
fty = -rcos ( 180 )
180 ……………………………………………………………. (5)
Where r is the distance between center of rotation and tool (in mm units), and is the angle between the P1 point and the X axis at the center of rotation (in units ). The combined speed «ft» according to (1), (2), (3), (4) and (5) is:
ft = ftx2 + fty2
= f
x2 — x c rsin ( 180 )
90 + ( r c 180 )2
x2 + c2 ……………….. (6)
Consequently, feedrate «f» designated by the program must be as follows:
f = ft
x2 + c2
x2 — x c rsin ( 180 )
90 + ( r c 180 )2
……………….. (7)
«ft» in formula (6) is the speed at the P1 point and the value of changes as the C axis rotates, which means that the value of «ft» will also change. Consequently, in order to keep the cutting feed «ft» as constant as possible the angle of rotation which is designated in one block must be reduced to as low as possible and the extent of the change in the value must be minimized.
7. Feed Functions 7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration
120
7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration
Function and purpose
This function performs acceleration and deceleration at a constant inclination during linear acceleration/deceleration in the rapid traverse mode. Compared to the method of acceleration /deceleration after interpolation, the constant inclination acceleration/deceleration method makes for improved cycle time.
Detailed description
(1) Rapid traverse constant inclination acceleration/deceleration are valid only for a rapid traverse
command. Also, this function is effective only when the rapid traverse command acceleration/deceleration mode is linear acceleration and linear deceleration.
(2) The acceleration/deceleration patterns in the case where rapid traverse constant inclination acceleration/deceleration are performed are as follows.
L
T s T s T d
T
Next block
rapid
rapid : Rapid traverse rate
Ts : Acceleration/deceleration time constant
Td : Command deceleration check time : Acceleration/deceleration inclination T : Interpolation time L : Interpolation distance
T = rapid
L +Ts
Td = Ts + (0~1.7 ms)
= tan-1 rapid
Ts ( )
rapid: Rapid traverse rate Ts: Acceleration/deceleration time constant Td: Command deceleration check time : Acceleration/deceleration inclination T: Interpolation time L: Interpolation distance
L
Ts Td
T
rapid
Next block
= tan-1 rapid Ts
( )
Td = + (0 ~ 1.7 ms) T 2
T = 2 Ts X L / rapid
7. Feed Functions 7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration
121
(3) When 2-axis simultaneous interpolation (linear interpolations) is performed during rapid
traverse constant inclination acceleration and deceleration, the acceleration (deceleration) time is the longest value of the acceleration (deceleration) times determined for each axis by the rapid traverse rate of commands executed simultaneously, the rapid traverse acceleration and deceleration time constant, and the interpolation distance, respectively. Consequently, linear interpolation is performed even when the axes have different acceleration and deceleration time constants.
<2-axis simultaneous interpolation (When linear interpolation is used, Tsx < Tsz, and Lx Lz)>
x Tsx Tsx
Tdx
Lx
Tx
Next block
X axis
Tsz
Lz
Tz
Z axis
rapid X
rapid Z
Z
Tsz Tdz
Next block
When Tsz is greater than Tsx, Tdz is also greater than Tdx, and Td = Tdz in this block.
(4) The program format of G0 (rapid traverse command) when rapid traverse constant inclination acceleration/deceleration are executed is the same as when this function is invalid (time constant acceleration/deceleration).
(5) This function is valid only for G0 (rapid traverse).
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration
122
7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration
Function and purpose
This function carries out the acceleration/deceleration according to the torque characteristic of the motor in the rapid traverse mode during automatic operation. (This function is not available in manual operation.) The rapid traverse constant inclination multi-step acceleration/deceleration method makes for improved cycle time because the positioning time is shortened by using the motor ability to its maximum. In general, the servomotor has the characteristic that the torque falls in the high-speed rotation range.
0 1000 3500
Rotation speed [r/min]
0
25
100
125
75
To rq
ue [N
m
]
50
2000 3000
(Note) This characteristic is data at input voltage 380VAC.
In the rapid traverse constant inclination acceleration/deceleration method, the acceleration has been treated constantly because this torque characteristic is not considered. So, It is necessary to use a minimum acceleration within the used speed range. Therefore, the margin of acceleration must be had in a low-speed range. Or if the acceleration is used to its maximum, the upper limit of the rotation speed must be slowed. Then, to use the servomotor ability to its maximum, acceleration/deceleration to which the torque characteristic is considered is carried out by the rapid traverse constant inclination multi-step acceleration/deceleration method. The acceleration/deceleration patterns in the case where rapid traverse constant inclination multi-step acceleration/deceleration are performed are as follows.
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration
123
Speed
Time
Acceler- ation
Time (b) Rapid traverse constant inclination
acceleration/deceleration
It was necessary to slow down the acceleration for high speed rotation.
tb
Speed
Time
Acceler- ation
Time
ta
(a) Rapid traverse constant inclination multi-step acceleration/deceleration
Number of steps is automatically adjusted by parameter setting.
Detailed description
(1) It is necessary to enable this function by set «2» to the parameter «#1205 G0bdcc».
However, note the following conditions. (a) «2» cannot be set to parameter «#1205 G0bdcc» besides the 1st part system. When «2» is
set for besides 1st part system, «Y51 parameter error 17» will occur. (b) When there is no specification for the rapid traverse constant inclination
acceleration/deceleration, «2» cannot be set to parameter «#1205 G0bdcc». Even if the parameter is set to «2», this function is invalid. A normal time constant acceleration/deceleration (acceleration/deceleration after interpolation) is applied.
(c) Even if «2» is set to «#1205 G0bdcc» when G00 non-interpolation type («#1086 G00Intp» = «1»), this function is invalid. In this case, a normal time constant acceleration/deceleration (acceleration/deceleration after interpolation) is applied.
(2) To use this function, the following parameters must be set for each axis.
#2001 rapid #2151 rated_spd #2153 G0t_rated #2152 acc_rate
Rapid traverse [mm/min] Rated speed [mm/min] Acceleration time to rated speed [ms] Acceleration at rapid traverse in ratio to the maximum acceleration [%]
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration
124
Max. acceleration
Acceleration at rapid traverse rate
Rapid traverse rate
Rated speed
Acceleration time to rated speed
Acceleration rate in proportion to the maximum acceleration rate Max. acceleration
Acceleration at rapid traverse rate =
Speed
Time
Acceleration
Time
(3) When either of the following conditions applies, this function is invalid and operates as «rapid
traverse constant inclination acceleration/deceleration». For the axis which the rapid traverse constant inclination multi-step acceleration/deceleration is not necessary for, set «0» to «#2151 rated_spd», «#2152 acc_rate» and «#2153 G0t_rated». (a) When «#2151 rated_spd» (rated speed) is «0» or larger than «#2001 rapid» (rapid traverse) (b) When «#2152 acc_rate» (Acceleration rate in proportion to the maximum acceleration rate)
is «0» or «100» (c) Even if «2» is set to «#1205 G0bdcc» when G00 non-interpolation type («#1086 G00Intp» =
«1»), this function is invalid. In this case, a normal time constant acceleration/deceleration (acceleration/deceleration after interpolation) is applied.
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration
125
(4) The comparison of the acceleration/deceleration patterns by the parameter setting is in the
table below.
Mode Rapid traverse constant
inclination multi-step acceleration/deceleration
#1086 G00Intp
#1205 G0bdcc Operation
0 Time constant acceleration/deceleration (interpolation type)
1 Constant inclination acceleration/deceleration (acceleration/deceleration before interpolation)
0
2 Constant inclination multi-step acceleration/deceleration
ON
1 Arbitrary Time constant acceleration/deceleration (non-interpolation type)
0 Time constant acceleration/deceleration (interpolation type)
1 Constant inclination acceleration/deceleration (acceleration/deceleration before interpolation)
0
2 Time constant acceleration/deceleration (interpolation type)
G00 command
OFF
1 Arbitrary Time constant acceleration/deceleration (non-interpolation type)
Manual rapid traverse
Arbitrary Arbitrary Arbitrary Time constant acceleration/deceleration (non-interpolation type)
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration
126
Detailed description (decision method of steps)
For rapid traverse constant inclination multi-step acceleration/deceleration, the number of steps is automatically adjusted by set parameter. The acceleration per step is assumed to be a decrease by 10% of the maximum acceleration per step. Therefore, the number of steps is decided as follows.
«Step» = (100 — «#2152 acc_rate») / 10 + 1 (Discard fractions less than 1) The acceleration/deceleration pattern when the parameter setting value is as follows is shown below.
No. Item Setting value 2001 rapid Rapid traverse rate 36000 [mm/min] 2151 rated_spd Rated speed 16800 [mm/min] 2152 acc_rate Acceleration rate in proportion to the
maximum acceleration rate 58 [%]
Acceleration
Speedrapid =36000
rated_spd =16800
amax
0.58amax
0.9amax 0.8amax
0.7amax
The acceleration decreases by 10% of the maximum acceleration amax.
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration
127
Detailed description (Acceleration pattern at two or more axis interpolation)
When there are two or more rapid traverse axes with a different acceleration pattern, there are the following two operation methods. Interpolation type (#1086 G0Intp = 0) : Moves from the start point to the end point by straight
line Non-interpolation type (#1086 G0Intp = 1) : Each axis moves severally at the speed of
the parameter Rapid traverse constant inclination multi-step acceleration/deceleration are valid only for an interpolation type. For the interpolation type, the acceleration pattern operates to the maximum acceleration within the range where tolerable acceleration of each axis is not exceeded.
(a) Acceleration pattern of X axis independently (b) Acceleration pattern of Y axis independently
Start point
End point
X
Y
4
3 5
Acceleration
Speed
ay
vy
Acceleration
Speed
ax
vx
Acceleration
Speed
Acceleration pattern when the axis moved to synthesis direction at X axis rapid traverse rate
Acceleration pattern of synthesis direction
(c) Acceleration pattern of synthesis direction
ax / 0.8 ay / 0.6
vy / 0.6 vx / 0.8
Acceleration pattern when the axis moved to synthesis direction at Y axis rapid traverse rate
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration
128
Detailed description (S-pattern filter control)
With S-pattern filter control, this enables the rapid traverse inclination multi-step acceleration/ deceleration fluctuation to further smoothen. This can be set in the range of 0 to 200 (ms) with the basic specification parameter «#1569 SfiltG0» (G00 soft acceleration/deceleration filter). With «#1570 Sfilt2» (Soft acceleration/deceleration filter 2), this also enables the acceleration/deceleration fluctuation to further smoothen.
Time
Speed
Parameter setting = SfiltG0 + Sfilt2
S-pattern filter
No S-pattern filter
Detailed description (Rapid traverse rate for the high-accuracy control mode)
The high-accuracy control mode’s rapid traverse rate («#2109 Rapid (H-precision)») can be set besides rapid traverse rate («#2001 rapid») during high-accuracy control, high-speed high-accuracy control I/II or high-accuracy spline control. Operation when the value is set at the high-accuracy control mode’s rapid traverse rate is as follows. (1) When «The high-accuracy control mode rapid traverse rate» > «rapid traverse rate»
This function is invalid and operates as «rapid traverse constant inclination acceleration/deceleration».
Rapid traverse
rate
Speed
Time Acceleration
Time
#2004 G0tL
(2) When «The high-accuracy control mode rapid traverse rate» < «rapid traverse rate»
«The high-accuracy control mode rapid traverse rate» is applied according to acceleration pattern calculated from acceleration rate to «rapid traverse», «rated speed», «G0 time constant to rated speed» and «maximum acceleration».
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration
129
Max. Acceleration
Acceleration at rapid traverse rate
Rapid traverse date
Rated speed
Acceleration time to rated speed
Speed
Time
Acceleration
Time
The high-accuracy control mode rapid traverse rate
Larger than the rated speed
Max. Acceleration
Acceleration at rapid traverse rate
Rapid traverse date
Rated speed
Acceleration time to rated speed
Speed
Time Acceleration
Time
The high-accuracy control mode rapid traverse rate
Smaller than the rated speed
Precautions
(1) Rapid traverse constant inclination multi-step acceleration/deceleration are valid only for a
rapid traverse command. Note that when the manual rapid traverse, rapid traverse constant inclination multi-step acceleration/deceleration cannot be used. In this case, a time constant acceleration/deceleration (acceleration/deceleration after interpolation) is applied. So, acceleration/deceleration is decided by the following parameters. #2001 rapid Rapid traverse rate #2003 smgst Acceleration/deceleration mode #2004 G0tL G0 time constant (linear) #2005 G0t1 G0 time constant (primary delay) The acceleration time (time constant) is different to the rapid traverse constant inclination multi-step acceleration/deceleration and the manual rapid traverse as shown in figure.
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration
130
Acceleration
Speed
Rapid traverse constant inclination multi-step acceleration/ deceleration
Manual rapid traverse (linear)
Time
Speed
Manual rapid traverse (linear)
Rapid traverse constant inclination multi-step acceleration/deceleration
S-pattern filter
Soft acceleration/deceleration
(2) Rapid traverse constant inclination multi-step acceleration/deceleration cannot be used in part
system excluding 1st part system. However, even if two or more part system is used, it is possible to use this function in case of the 1st part system.
(3) When there is no specification for the rapid traverse constant inclination acceleration/deceleration, this function is invalid even if «2» is set to parameter «#1205 G0bdcc». In this case, a normal time constant acceleration/deceleration (acceleration/deceleration after interpolation) is applied.
(4) When G00 non-interpolation type («#1086 G00Intp» = «1»), rapid traverse constant inclination multi-step acceleration/deceleration cannot be used. It is valid at interpolation mode only.
(5) When the rapid traverse constant inclination multi-step acceleration/deceleration is applied, rapid traverse acceleration/deceleration types («#2003 smgst» bit0 to bit3) are ignored.
(6) When the rapid traverse constant inclination multi-step acceleration/deceleration is valid, G0 constant inclination («#1200 G0_acc») cannot be used. Even if G0 constant inclination is valid («#1200 G0_acc» = 1), the setting is ignored.
(7) When the rapid traverse constant inclination multi-step acceleration/deceleration is valid, programmable in-position check cannot be used. The in-position width will be ignored even if commanded.
(8) This function cannot be used during the tool center point control. (9) For rapid traverse constant inclination multi-step acceleration/deceleration, feedforward
control is invalid.
7. Feed Functions 7.9 Exact Stop Check; G09
131
7.9 Exact Stop Check; G09 Function and purpose
In order to prevent roundness during corner cutting and machine shock when the tool feedrate changes suddenly, there are times when it is desirable to start the commands in the following block once the in-position state after the machine has decelerated and stopped or the elapsing of the deceleration check time has been checked. The exact stop check function is designed to accomplish this purpose. Either the deceleration check time or in-position state is selected with parameter «#1193 inpos». In-position check is valid when «#1193 inpos» is set to 1. The in-position width is set with parameter «#2224 SV024» on the servo parameter screen by the machine manufacturer.
Command format
G09 ;
The exact stop check command G09 has an effect only with the cutting command (G01 — G03) in its particular block.
Example of program
N001 G09 G01 X100.000 F150 ; The following block is started once the deceleration
check time or in-position state has been checked after the machine has decelerated and stopped.
N002 Y100.000 ;
X axis
f (Commanded speed)
Time
Solid line indicates speed pattern with G09 command. Broken line indicates speed pattern without G09 command.
Fig. 1 Exact stop check result
Y axis
N002
N001
Tool
With G09
Without G09
N001
N002
7. Feed Functions 7.9 Exact Stop Check; G09
132
Detailed description
(1) With continuous cutting feed
Ts
Fig. 2 Continuous cutting feed command
Previous block Next block
(2) With cutting feed in-position check
Fig. 3 Block joint with cutting feed in-position check
Ts Ts
Previous block Next block
Lc (in-position width)
In Figs. 2 and 3:
Ts = Cutting feed acceleration/deceleration time constant Lc = In-position width As shown in Fig. 3, the remaining distance (shaded area in Fig. 3) of the previous block when the next block is started can be set into the servo parameter «#2224 SV024» as the in-position width «Lc». The in-position width is designed to reduce the roundness at the workpiece corners to below the constant value.
Lc Next block
Previous block
To eliminate corner roundness, set the value as small as possible to servo parameter «#2224 SV024» and perform an in-position check or assign the dwell command (G04) between blocks.
7. Feed Functions 7.9 Exact Stop Check; G09
133
(3) With deceleration check
(a) With linear acceleration/deceleration
Ts
Td
Previous block Next block
Ts : Acceleration/deceleration time constant Td : Deceleration check time Td = Ts + ( 0 ~ 14ms)
(b) With exponential acceleration/deceleration
Ts
Td
Previous block Next block
Ts : Acceleration/deceleration time constant Td : Deceleration check time Td = 2 Ts + ( 0 ~ 14ms)
(c) With exponential acceleration/linear deceleration
2 x Ts
Td Ts
Previous block Next block
Ts : Acceleration/deceleration time constant Td : Deceleration check time Td = 2 Ts + ( 0 ~ 14ms)
The time required for the deceleration check during cutting feed is the longest among the cutting feed deceleration check times of each axis determined by the cutting feed acceleration/deceleration time constants and by the cutting feed acceleration/ deceleration mode of the axes commanded simultaneously. (Note 1) To execute exact stop check in a fixed cycle cutting block, insert command G09
into the fixed cycle subprogram.
7. Feed Functions 7.10 Exact Stop Check Mode; G61
134
7.10 Exact Stop Check Mode; G61
Function and purpose
Whereas the G09 exact stop check command checks the in-position status only for the block in which the command has been assigned, the G61 command functions as a modal. This means that deceleration will apply at the end points of each block to all the cutting commands (G01 to G03) subsequent to G61 and that the in-position status will be checked. G61 is released by high-accuracy control (G61.1), automatic corner override (G62), tapping mode (G63), or cutting mode (G64).
Command format
G61 ;
In-position check is executed in the G61 block, and thereafter, the in-position check is executed at the end of the cutting command block is executed until the check mode is canceled.
7.11 Deceleration Check Function and purpose
The deceleration check is a function that determines the method of the check at the completion of the axis movement block’s movement. The deceleration check includes the in-position check and commanded speed check method. The G0 and G1 deceleration check method combination can be selected. (Refer to section «Deceleration check combination».) With this function, the deceleration check in the reverse direction of G1 G0 or G1 G1 can be changed by changing the parameter setting. (1) Types of deceleration check
Commanded speed check
With the commanded speed check, the completion of deceleration is judged when the command to the motor is completed
Judges the stop here Deceleration start point
Command to motor
movement of motor
In-position check With the in-position check, the completion of deceleration is judged when the motor moves to the in-position width designated with the parameter.
Judges the stop here
G0/G1 in-position width
Deceleration start point
7. Feed Functions 7.11 Deceleration Check
135
(2) Designating deceleration check
The deceleration check by designating a parameter includes «deceleration check specification type 1» and «deceleration check specification type 2». The setting is selected with the parameter «#1306 InpsTyp».
(a) Deceleration check specification type 1 («#1306 InpsTyp» = 0) The G0 and G1 deceleration check method can be selected with the base specification
parameter deceleration check method 1 (#1193 inpos) and «deceleration check method 2» (#1223 aux07/bit1).
Parameter Rapid traverse command Parameter Other than rapid traverse command
(G1 : other than G0 command) inpos
(#1193) G0XX
(G0+G9XX) AUX07/BIT-1 (#1223/BIT-1) G1+G9XX G0XX
0 Command
deceleration check
0 Command
deceleration check
1 In-position check 1 In-position
check
No deceleration check
(Note 1) XX expresses all commands.
(Note 2) «#1223 aux07» is the part system common parameter.
(b) Deceleration check specification type 2 («#1306 InpsTyp» = 1) Rapid traverse and cutting in-position are designated with the «#1193 inpos» parameter.
Parameter Command block #1193 Inpos G0 G1+G9 G1
0 Command deceleration check
Command deceleration check
No deceleration check
1 In-position check
In-position check
No deceleration check
(Note 1) «#1193 inpos» is the parameter per part system.
(Note 2) «G0» means the rapid traverse, and «G1» means the cutting feed.
7. Feed Functions 7.11 Deceleration Check
136
7.11.1 G1 G0 Deceleration Check
Detailed operations
(1) In G1 G0 continuous blocks, the parameter «#1502 G0Ipfg» can be changed to change the
deceleration check in the reverse direction. Same direction Reverse direction
G0Ipfg: 0
G0Ipfg: 1
Command deceleration
Example of program
When there is a deceleration check in the movement of several axes: (1) G91 G1 X100. Y100. F4000 ;
G0 X-100. Y120. ; A deceleration check is carried out, because the X axis moves in the reverse direction in the program above.
(2) G91 G1 X100. Y-100. F4000 ;
G0 X80. Y100. ; A deceleration check is carried out, because the Y axis moves in the reverse direction in the program above.
(3) G90 G1 X100. Y100. F4000 ;
G0 X80. Y120. ; A deceleration check is carried out, because the X axis moves in the reverse direction in the program above. (When the program start position is X0 Y0)
(4) G91 G1 X100. Y100. F4000 ;
G0 X100. Y100. ; A deceleration check is not carried out, because both the X axis and the Y axis move in the same direction in the program above.
(5) G91 G1 X100. Y80. F4000 ;
G0 X80. ; A deceleration check is not carried out, because the X axis moves in the same direction, and there is no Y axis movement command in the program above.
G0 G1
G0 G1
G1 G0
G1 G0
7. Feed Functions 7.11 Deceleration Check
137
7.11.2 G1 G1 Deceleration Check Detailed operations
(1) In G1 G1 continuous blocks, the parameter «#1503 G1Ipfg» can be changed to change the
deceleration check of the reverse direction. Same direction Reverse direction
G1Ipfg: 0
G1Ipfg: 1
Command deceleration
Example of program
When there is a deceleration check in the movement of several axes: (1) G91 G1 X100. Y100. F4000 ;
G1 X-100. Y120. ; A deceleration check is carried out, because the X axis moves in the reverse direction in the program above.
(2) G91 G1 X100. Y-100. F4000 ;
G1 X80. Y100. ; A deceleration check is carried out, because the Y axis moves in the reverse direction in the program above.
(3) G90 G1 X100. Y100. F4000 ;
G1 X80. Y120. ; A deceleration check is carried out, because the X axis moves in the reverse direction in the program above. (When the program start position is X0 Y0)
(4) G91 G1 X100. Y100. F4000 ;
G1 X100. Y100. ; A deceleration check is not carried out, because both the X axis and the Y axis move in the same direction in the program above.
(5) G91 G1 X100. Y80. F4000 ;
G1 X80. ; A deceleration check is not carried out, because the X axis moves in the same direction, and there is no Y axis movement command in the program above.
G1 G1
G1 G1
G1 G1
G1 G1
7. Feed Functions 7.12 Automatic Corner Override; G62
138
7.12 Automatic Corner Override; G62
Function and purpose
With tool radius compensation, this function reduces the load during inside cutting of automatic corner R, or during inside corner cutting, by automatically applying override to the feed rate. Automatic corner override is valid until the tool radius compensation cancel (G40), exact stop check mode (G61), high-accuracy control mode (G61.1), tapping mode (G63), or cutting mode (G64) command is issued.
Command format
G62 ;
Machining inside corners
When cutting an inside corner as in Fig. 1, the machining allowance amount increases and a greater load is applied to the tool. To remedy this, override is applied automatically within the corner set range, the feedrate is reduced, the increase in the load is reduced and cutting is performed effectively. However, this function is valid only when finished shapes are programmed.
workpiece Machining allowance
Programmed path (finished shape)
Workpiece surface shape
Tool center path
Tool
: Max. angle at inside corner Ci : Deceleration range (IN)
Machining allowance
Ci
S
(1) (2) (3)
Deceleration
Fig.1
range
7. Feed Functions 7.12 Automatic Corner Override; G62
139
(1) Operation
(a) When automatic corner override is not to be applied : When the tool moves in the order of (1) (2) (3) in Fig. 1, the machining allowance at (3) increases by an amount equivalent to the area of shaded section S and so the tool load increases.
(b) When automatic corner override is to be applied : When the inside corner angle in Fig. 1 is less than the angle set in the parameter, the override set into the parameter is automatically applied in the deceleration range Ci.
(2) Parameter setting
The following parameters are set into the machining parameters : # Parameter Setting range
#8007 OVERRIDE 0 to 100% #8008 MAX ANGLE 0 to 180 #8009 DSC. ZONE 0 to 99999.999mm or 0 to 3937.000 inches
Refer to the Instruction Manual for details on the setting method.
Automatic corner R
Workpiece
P ro
gr am
m ed
pa
th
M ac
hi ni
ng
al lo
w an
ce
W or
k su
rfa ce
sh
ap e
To ol
c en
te r
pa th
Corner R section
Machining allowance
Corner R center
Ci
(1) The override set in the parameter is automatically applied at the deceleration range Ci and
corner R section for inside offset with automatic corner R. (There is no angle check.)
7. Feed Functions 7.12 Automatic Corner Override; G62
140
Example of operations
(1) Line — line corner
Tool
Program
Tool center
Ci
The override set in the parameter is applied at Ci.
(2) Line — arc (outside) corner
Tool
Program Tool center
Ci
The override set in the parameter is applied at Ci.
(3) Arc (inside compensation) — line corner
Tool
Program
Ci
Tool
Tool center
The override set in the parameter is applied at Ci. (Note) The deceleration range Ci where the override is applied is the length of the arc with an
arc command.
(4) Arc (inside compensation) — arc (outside compensation) corner
Program
Tool center
N1
Ci N2
The override set in the parameter is applied at Ci.
7. Feed Functions 7.12 Automatic Corner Override; G62
141
Relation with other functions
Function Override at corner
Cutting feed override Automatic corner override is applied after cutting feed override has been applied.
Override cancel Automatic corner override is not canceled by override cancel.
Speed clamp Valid after automatic corner override
Dry run Automatic corner override is invalid.
Synchronous feed Automatic corner override is applied to the synchronous feedrate.
Thread cutting Automatic corner override is invalid.
G31 skip Program error results with G31 command during tool radius compensation.
Machine lock Valid
Machine lock high speed Automatic corner override is invalid.
G00 Invalid
G01 Valid
G02, G03 Valid
7. Feed Functions 7.12 Automatic Corner Override; G62
142
Precautions
(1) Automatic corner override is valid only in the G01, G02, and G03 modes; it is not effective in
the G00 mode. When switching from the G00 mode to the G01 (or G02 or G03) mode at a corner (or vice versa), automatic corner override will not be applied at that corner in the G00 block.
(2) Even if the automatic corner override mode is entered, the automatic corner override will not be
applied until the tool radius compensation mode is entered. (3) Automatic corner override will not be applied on a corner where the tool radius compensation is
started or canceled. Start-up block Program
Cancel block
Automatic corner override will not be applied
Tool center
(4) Automatic corner override will not be applied on a corner where the tool radius compensation I,
K vector command is issued.
Block containing I, K vector command
Program
Tool center
Automatic corner override will not be applied (G41X_Z_I_K_;)
(5) Automatic corner override will not be applied when intersection calculation cannot be
executed. Intersection calculation cannot be executed in the following case.
(a) When the movement command block does not continue for four or more times.
(6) The deceleration range with an arc command is the length of the arc. (7) The inside corner angle, as set by parameter, is the angle on the programmed path. (8) Automatic corner override will not be applied when the maximum angle in the parameter is set
to 0 or 180. (9) Automatic corner override will not be applied when the override in the parameter is set to 0 or
100.
7. Feed Functions 7.13 Tapping Mode; G63
143
7.13 Tapping Mode; G63
Function and purpose
The G63 command allows the control mode best suited for tapping to be entered, as indicated below : (1) Cutting override is fixed at 100%. (2) Deceleration commands at joints between blocks are invalid. (3) Feed hold is invalid. (4) Single block is invalid. (5) In-tapping mode signal is output. G63 is released by the exact stop check mode (G61), high-accuracy control mode (G61.1), automatic corner override (G62), or cutting mode (G64).
Command format
G63 ;
7.14 Cutting Mode ; G64
Function and purpose
The G64 command allows the cutting mode in which smooth cutting surfaces are obtained to be established. Unlike the exact stop check mode (G61), the next block is executed continuously with the machine not decelerating and stopping between cutting feed blocks in this mode. G64 is released by the exact stop mode (G61), high-accuracy control mode (G61.1), automatic corner override (G62), or tapping mode (G63). This cutting mode is established in the initialized status.
Command format
G64 ;
8. Dwell 8.1 Per-second Dwell ; G04
144
8. Dwell
The G04 command can delay the start of the next block. 8.1 Per-second Dwell ; G04
Function and purpose
The machine movement is temporarily stopped by the program command to make the waiting time state. Therefore, the start of the next block can be delayed. The waiting time state can be canceled by inputting the skip signal.
Command format
G04 X__ ; or G04 P__ ; X, P Dwell time
The input command unit for the dwell time depends on the parameter.
Detailed description
(1) When designating the dwell time with X, the decimal point command is valid.
(2) When designating the dwell time with P, the availability of the decimal point command can be selected with the parameter (#8112). When the decimal point command is invalid in the parameter setting, the command below the decimal point issued with P is ignored.
(3) When the decimal point command is valid or invalid, the dwell time command range is as follows.
Command range when the decimal point command is valid
Command range when the decimal point command is invalid
0 ~ 99999.999 (s) 0 ~ 99999999 (ms)
(4) The dwell time setting unit applied when there is no decimal point can be made 1s by setting 1 in the parameter #1078 Decpt2. This is effect only for X and P for which the decimal command is valid.
(5) When a cutting command is in the previous block, the dwell command starts calculating the dwell time after the machine has decelerated and stopped. When it is commanded in the same block as an M, S, T or B command, the calculation starts simultaneously.
(6) The dwell is valid during the interlock.
(7) The dwell is valid even for the machine lock.
(8) The dwell can be canceled by setting the parameter #1173 dwlskp beforehand. If the set skip signal is input during the dwell time, the remaining time is discarded, and the following block will be executed.
Previous block cutting command
Next block
Dwell command
Dwell time
8. Dwell 8.1 Per-second Dwell ; G04
145
Example of program
Dwell time [sec]
#1078 Decpt2 = 0 #1078 Decpt2 = 1 Command DECIMAL
PNT-N DECIMAL
PNT-P DECIMAL
PNT-N DECIMAL
PNT-P G04 X500 ; 0.5 500 G04 X5000 ; 5 5000 G04 X5. ; 5 5 G04 X#100 ; 1000 1000 G04 P5000 ; 5 5 5000 G04 P12.345 ; 0.012 12.345 0.012 12.345 G04 P#100 ; 1 1000 1 1000
(Note 1) The above examples are the results under the following conditions. Input setting unit 0.001mm or 0.0001inch #100 = 1000 ; (Note 2) «DECIMAL PNT-P» is a control parameter (#8112). (Note 3) If the input setting unit is 0.0001inch, the X before G04 will be multiplied by 10. For
example for «X5. G04 ;», the dwell time will be 50 sec. Precautions and restrictions
(1) When using this function, command X after G04 in order to make sure that the dwell is based
on X.
9. Miscellaneous Functions 9.1 Miscellaneous Functions (M8-digits BCD)
146
9. Miscellaneous Functions 9.1 Miscellaneous Functions (M8-digits BCD)
Function and purpose
The miscellaneous (M) functions are also known as auxiliary functions, and they include such numerically controlled machine functions as spindle forward and reverse rotation, operation stop and coolant ON/OFF. These functions are designated by an 8-digit number (0 to 99999999) following the address M with this controller, and up to 4 groups can be commanded in a single block. (Example) G00 Xx Mm1 Mm2 Mm3 Mm4 ;
When five or more commands are issued, only the last four will be valid. The output signal is an 8-digit BCD code and start signal. The eight commands of M00, M01, M02, M30, M96, M97, M98 and M99 are used as auxiliary commands for specific objectives and so they cannot be used as general auxiliary commands. This therefore leaves 94 miscellaneous functions which are usable as such commands. Reference should be made to the instructions issued by the machine manufacturer for the actual correspondence between the functions and numerical values. When the M00, M01, M02, and M30 functions are used, the next block is not read into the pre-read buffer due to pre-read inhibiting. If the M function is designated in the same block as a movement command, the commands may be executed in either of the following two orders. Which of these sequences actually applies depends on the machine specifications.
(1) The M function is executed after the movement command.
(2) The M function is executed at the same time as the movement command.
Processing and completion sequences are required in each case for all M commands except M96, M97, M98 and M99. The 8M functions used for specific purposes will now be described.
Program stop : M00
When the tape reader has read this function, it stops reading the next block. As far as the NC system’s functions are concerned, only the tape reading is stopped. Whether such machine functions as the spindle rotation and coolant supply are stopped or not differs according to the machine in question. Re-start is enabled by pressing the automatic start button on the machine operation board. Whether resetting can be initiated by M00 depends on the machine specifications.
9. Miscellaneous Functions 9.1 Miscellaneous Functions (M8-digits BCD)
147
Optional stop ; M01
If the tape reader reads the M01 command when the optional stop switch on the machine operation board is ON, it will stop and the same effect as with the M00 function will apply. If the optional stop switch is OFF, the M01 command is ignored. (Example)
: N10 G00 X1000 ; N11 M01 ; N12 G01 X2000 Z3000 F600 ; :
Optional stop switch status and operation Stops at N11 when switch is ON Next command (N12) is executed
without stopping at N11 when switch is OFF
Program end ; M02 or M30
This command is normally used in the final block for completing the machining, and so it is primarily used for tape rewinding. Whether the tape is actually rewound or not depends on the machine specifications. Depending on the machine specifications, the system is reset by the M02 or M30 command upon completion of tape rewinding and any other commands issued in the same block. (Although the contents of the command position display counter are not cleared by this reset action, the modal commands and compensation amounts are canceled.) The next operation stops when the rewinding operation is completed (the in-automatic operation lamp goes off). To restart the unit, the automatic start button must be pressed or similar steps must be taken. When the program is restarted after M02 and M30 are completed, if the first movement command is designated only with a coordinate word, the interpolation mode will function when the program ends. It is recommended that a G function always be designated for the movement command designated first. (Note 1) Independent signals are also output respectively for the M00, M01, M02 and M30
commands and these outputs are each reset by pressing the reset key. (Note 2) M02 or M30 can be assigned by manual data input (MDI). At this time, commands can be
issued simultaneously with other commands just as with the tape.
Macro interrupt ; M96, M97
M96 and M97 are M codes for user macro interrupt control. The M code for user macro interrupt control is processed internally, and is not output externally. To use M96 and M97 as an auxiliary code, change the setting to another M code with the parameter (#1109 subs_M and #1110 M96_M, #1111 M97_M).
Subprogram call/completion ; M98, M99
These commands are used as the return instructions from branch destination subprograms and branches to subprograms. M98 and M99 are processed internally and so M code signals and strobe signals are not output.
Internal processing with M00/M01/M02/M30 commands
Internal processing suspends pre-reading when the M00, M01, M02 or M30 command has been read. Other tape rewinding operations and the initialization of modals by resetting differ according the machine specifications.
9. Miscellaneous Functions 9.2 Secondary Miscellaneous Functions (B8-digits, A8 or C8-digits)
148
9.2 Secondary Miscellaneous Functions (B8-digits, A8 or C8-digits)
Function and purpose
These serve to assign the indexing table positioning and other such functions. In this controller, they are assigned by an 8-digit number from 0 to 99999999 following address A, B or C. The machine maker determines which codes correspond to which positions. If the A, B or C function is designated in the same block as a movement command, the commands may be executed in either of the following two orders. The machine specifications determine which sequence applies.
(1) The A, B or C function is executed after the movement command.
(2) The A, B or C function is executed simultaneously with the movement command.
Processing and completion sequences are required for all secondary miscellaneous functions. The table below given the various address combinations. It is not possible to use an address which is the same for the axis name of an additional axis and secondary miscellaneous function.
Additional axis name 2nd miscellaneous function
A B C
A B C
(Note) When A has been assigned as the secondary miscellaneous function address, the following commands cannot be used.
(1) Linear angle commands (,A can be used.) (2) Geometric commands
9. Miscellaneous Functions 9.3 Index Table Indexing
149
9.3 Index Table Indexing Function and purpose
Index table indexing can be carried out by setting the index axis. The indexing command only issues the indexing angle to the axis set for indexing. It is not necessary to command special M codes for table clamping and unclamping, thus simplifying the program.
Detailed description
The index table index function carries out operations as follows.
(Example) G00 B90 ;
The axis that was designated as the index axis with parameter «#2076 index x».
(1) Set the «index_x» parameter (#2076) for the axis in which index table indexing will be carried out to «1».
(2) The movement command (either absolute or incremental) for the selected axis is executed with the program command.
(3) An unclamp process are carried out before the axis movement.
(4) The commanded axis movement starts after the unclamp process completes.
(5) The clamp process is carried out after the movement is completed.
(6) The next block is processed after the unclamp process completes.
T10 FIN WAIT 0800 T10 FIN WAIT 0800
B axis movement
Unclamp completed
Unclamp command
G0 B90. ;Program command
9. Miscellaneous Functions 9.3 Index Table Indexing
150
Precautions
(1) Several axes can be set as index table indexing axes.
(2) The movement speed of index table indexing axes follows the feedrate of the modal (G0/G1) at that time.
(3) The unclamp process for the indexing axes is also issued when the index table indexing axes are commanded in the same block as other axes. Thus, the movement of other axes commanded in the same block is not carried out until the unclamp process completes.
Note that the movement of other axes commanded in the same block is carried out for non-interpolation commands.
(4) Index table indexing axes are used as normal rotation axes, but this function performs an unclamp process even for linear axes.
(5) If some error that makes unclamp command OFF occurs during indexing axis movement in automatic operation, the unclamp state will be remained, and the indexing axis will execute a deceleration stop.
Other axes commanded in the same block will also execute a deceleration stop, except for non-interpolation commands.
(6) If the axis movement is interrupted by an interlock, etc., during indexing axis movement, the unclamp state will be remained.
(7) The clamp and unclamp process are not executed when the movement commands of the index table indexing axis are continuous.
Note that the clamp and unclamp process are executed even when the movement commands are continued during single block operation.
(8) Make sure that the command position is at a position where clamping is possible.
10. Spindle Functions 10.1 Spindle Functions (S6-digits Analog)
151
10. Spindle Functions 10.1 Spindle Functions (S6-digits Analog)
Function and purpose
When the S6-digits function is added, a 6-digit value (0 to 999999) can be designated after the S code. Always select S command binary output when using this function. If the S function is designated in the same block as a movement command, the commands may be executed in either of the following two orders. The machine specifications determine which one is applied. (1) The S function is executed after the movement command. (2) The S function is executed simultaneously with the movement command. By assigning a 6-digit number following the S code, these functions enable the appropriate gear signals, voltages corresponding to the commanded spindle speed (r/min) and start signals to be output. If the gear step is changed manually other than when the S command is being executed, the voltage will be obtained from the set speed at that gear step and the previously commanded speed, and then will be output. The analog signal specifications are given below.
(1) Output voltage …………… 0 to 10V
(2) Resolution…………………. 1/4096 (2-12)
(3) Load conditions …………. 10k
(4) Output impedance ……… 220 If the parameters for up to 4 gear stages are set in advance, the gear stage corresponding to the S command will be selected and the gear signal will be output. The analog voltage is calculated in accordance with the input gear signal. (1) Parameters corresponding to individual gears …….Limit rotation speed, maximum rotation
speed, shift rotation speed, tap rotation speed.
(2) Parameters corresponding to all gears……………….Minimum rotation speed, orientation rotation speed
10.2 Spindle Functions (S8-digits)
Function and purpose
These functions are assigned with an 8-digit (0 to 99999999) number following the address S, and one group can be assigned in one block. The output signal is a 32-bit binary data with sign and start signal. Processing and completion sequences are required for all S commands.
10. Spindle Functions 10.3 Constant Surface Speed Control; G96, G97
152
10.3 Constant Surface Speed Control; G96, G97 10.3.1 Constant Surface Speed Control
Function and purpose
These cinommands automatically control the spindle speed in line with the changes in the radius coordinate values as cutting proceeds in the diametrical direction, and they serve to keep the cutting pot speed constant during the cutting.
Command format
G96 S__ P__; Constant surface speed ON
S : Peripheral speed P : Constant surface speed control axis
G97 ; Constant surface speed cancel
Detailed description
(1) The constant surface speed control axis is set by parameter «#1181 G96_ax».
0 : Fixed at 1st axis (P command invalid) 1 : 1st axis 2 : 2nd axis 3 : 3rd axis
(2) When the above-mentioned parameter is not zero, the constant surface speed control axis can be assigned by address P. (Example) G96_ax : 1
Program Constant surface speed control axis G96 S100 ; 1st axis G96 S100 P3 ; 3rd axis
(3) Example of selection program and operation
G90 G96 G01 X50. Z100. S200 ;
~ G97 G01 X50. Z100. F300 S500 ;
~ M02 ;
The spindle speed is controlled so that the peripheral speed is 200m/min.
The spindle speed is controlled to 500r/min.
The modal returns to the initial setting.
10. Spindle Functions 10.4 Spindle Clamp Speed Setting; G92
153
10.4 Spindle Clamp Speed Setting; G92
Function and purpose
The maximum clamp speed of the spindle can be assigned by address S following G92 and the minimum clamp speed by address Q.
Command format
G92 S__ Q__;
S : Maximum clamp speed Q : Minimum clamp speed
Detailed description
(1) Besides this command, parameters can be used to set the rotational speed range up to 4
stages in 1 r/min units to accommodate gear selection between the spindle and spindle motor. The lowest upper limit and highest lower limit are valid among the rotational speed ranges based on the parameters and based on G92 Ss Qq ;
(2) Set in the parameter «#1146 Sclamp» or «#1227 aux11/bit5» whether to carry out rotation speed clamp only in the constant surface speed mode or even when the constant surface speed is canceled.
(Note1) G92S command and speed clamp operation
Sclamp = 0 Sclamp = 1 aux11/bit5 = 0 aux11/bit5 = 1 aux11/bit5 = 0 aux11/bit5 = 1
In G96 SPEED CLAMP COMMAND SPEED CLAMP COMMAND Command
In G97 SPINDLE SPEED COMMAND SPEED CLAMP COMMAND In G96 SPEED CLAMP EXECUTION SPEED CLAMP EXECUTION
Operation In G97 NO SPEED CLAMP SPEED CLAMP
EXECUTION NO SPEED CLAMP
(Note2) The address Q following the G92 command is handled as the spindle speed clamp speed regardless of the constant surface mode.
(3) The command value of spindle clamp speed will be cleared by modal reset (reset2 or reset & rewind). Note that the modal is retained if the parameter #1210 RstGmd / bit19 is ON.
Precautions
(1) Once the maximum clamp speed and the minimum clamp speed are set, the maximum clamp speed will
not be canceled even if the command such as G92 S0 is issued. Even when G92 S0 is commanded, the value of Qq is kept valid and S value (S0) falls below Q value (Qq). Thus, Qq will be handled as the maximum clamp speed and S0 as the minimum clamp speed.
10. Spindle Functions 10.5 Spindle/C Axis Control
154
10.5 Spindle/C Axis Control
Function and purpose
This function enables one spindle (MDS-A/B-SP and later) to also be used as a C axis (rotation axis) by an external signal.
Detailed description
(1) Spindle/C axis changeover
Changeover between the spindle and C axis is done by the C axis SERVO ON signal.
At servo OFF ……………..Spindle (C axis control not possible) At servo ON ……………….C axis (spindle control not possible)
The C axis is in a reference position return incomplete state.
C axis Spindle Spindle Servo ON
Reference position return state Reference position return is incomplete when the Z phase has not been passed. Reference position return is complete when the Z phase has been passed. C axis position data The NC’s internal C axis position data is updated even for the spindle rotation
during spindle control. The C axis coordinate position counter is held during spindle control, and is
updated for the amount moved during spindle control when the C axis servo READY is turned ON. (The C axis position at servo ON may differ from the position just before the previous servo OFF.)
(2) Changeover timing chart example
2
Reference position return complete status
Blocks being calculated
Recalculation request
Blocks being executed
C axis command (automatic operation)
Spindle forward run/ reverse run start
Servo ON
Servo READY
Motor speed C axis movement
Program error (P430)
Reference position return complete
Reference position return complete
Orientation Orientation
Spindle reverse run
Reverse run
2 1
1
Forward run
Spindle forward run
C axis command
Servo ON C axis command C axis command
recalculation
Servo OFF
Spindle reverse run
C axis command
Spindle forward Spindle reverse run Servo ON Servo OFF Servo ON
Servo ON
Program error because the reference position return is incomplete at this calculation.
Reference position return complete at recalculation
10. Spindle Functions 10.5 Spindle/C Axis Control
155
(Note) For axis commands, the reference position return complete is checked at calculation.
Thus, when the C axis servo ON command and C axis command are continuous, the program error (P430) occur as shown above in 2. In response to this kind of situation, the following two processes must be carried out on user PLC, as shown above in 1. Input the recalculation request signal with a servo ON command. Wait for the completion of the servo ON command until the C axis enters a servo
READY state. (3) C axis gain
The C axis gain is changed over (the optimum gain is selected) by the C axis cutting condition. During C axis cutting feed, cutting gain is applied. During other axis’ cutting feed (C axis face turning), non-cutting stop gain is applied. Non-cutting gain is applied in all other cases.
Z axis command (other part system)
X axis command (C axis part system)
Selected gain
C axis command
Non-cutting gain
Non-cutting gainNon-cutting gain Cutting stop gain Cutting gain
G1
G1
G1 G0
G0
G1
G0
G0
(Note 1) The cutting feed of other part systems does not affect the C axis gain selection. (Note 2) There are 1st to 3rd cutting gains, which are selected with the ladder.
(4) Deceleration check in movement including spindle/C-axis The deceleration check in a movement command including the spindle/C-axis is as the table described below when the following condition is fulfilled.
When the different values are set for the position loop gain in non-cutting mode (spindle parameter #3203 PGCO) and the position loop gain in cutting mode (spindle parameter #3330 PGC1 to #3333 PGC4).
That is because a vibration and so on occurs in the machine when the gain is changed during the axis movement.
Parameter Rapid traverse command Parameter Other than rapid traverse command
(G1 : other than G0 command) Inpos
(#1193) G0XX
(G0+G9XX) AUX07/BIT-1 (#1223/BIT-1)
G1+G9XX (G1+G9XX) G1 G1
0 Command
deceleration check
0
1 In-position check 1
In-position check
(Applicable only to SV024)
No deceleration check
(Note 1) When G1 command is issued, the in-position check is performed regardless of the deceleration check parameter.
(Note 2) XX expresses all commands.
10. Spindle Functions 10.5 Spindle/C Axis Control
156
Precautions and Restrictions
(1) A reference position return cannot be executed by the orientation when there is no Z phase in
the detector (PLG, ENC, other). Replace the detector with one having a Z phase, or if using the detector as it is, set the position control changeover to «After deceleration stop» in the parameters (Spindle parameters, SP129 bitE: 1), and set the axis to «Axis without zero point» (Zero point return parameters, noref: 1).
(2) The program error (P430) will occur if a C axis command is issued during servo OFF or during orientation.
(3) Do not execute a servo OFF during a C axis command. The remaining C axis commands will be cleared at servo ON. (If servo OFF is executed during C axis control, the feed will stop and spindle control will occur.)
(4) If servo ON is executed during spindle rotation, the rotation will stop and C axis control will occur.
(5) Dog-type reference position return are not possible for the C axis. Set the reference position return to the orientation method in the parameters (Spindle parameters, SP129 bitE: 0), or set the axis to «Axis without zero point» (Zero point return parameters, noref: 1).
10. Spindle Functions 10.6 Multiple Spindle Control
157
10.6 Multiple Spindle Control
Function and purpose
Multiple spindle control is a function used to control the sub-spindle in a machine tool that has a main spindle (1st spindle) and a sub-spindle (2nd spindle to 4th spindle).
Multiple spindle control II: (ext36/bit0 = 1)
Control following the external signal (spindle command selection signal, spindle selection signal) and spindle control command ([S ;] only), etc. The spindle selection command [S = ;] cannot be used.
10. Spindle Functions 10.6 Multiple Spindle Control
158
10.6.1 Multiple Spindle Control II
Function and purpose
Multiple spindle control II is a function that designates which spindle to select with the signals from PLC. The command is issued to the spindle with one S command.
Detailed description
(1) Spindle command selection, spindle selection
The S command to the spindle is output as the rotation speed command to the selected spindle when the spindle selection signal (SWS) from the PLC turns ON. The selected spindle rotates at the output rotation speed. The spindle whose selection is canceled when the spindle selection signal (SWS) turns OFF maintains the speed at which it was rotating at before being canceled. This allows each axis to be simultaneously rotated at differing rotation speeds. The spindle command selection signal is used to determine which part system each spindle receives the S command from.
S command $2 S command $1
Y18A8 Y1894
Y1908
Y1968
Y19C8
1st spindle
R6500/6501
R6550/6551 Y18F4
2nd spindle
Y1954 3rd spindle
R6600/6601
R6650/6651 Y19B4
4th spindle
X18A0
X1900
X1960
X19C0
R7002
R7052
R7102
R7152
Encoder input $2
Encoder input $1
R2567
R2767
R7000/7001
R7050/7051
R7100/7101
R7150/7151
PLC side
PLC side
PLC side
PLC side
Spindle rotation speed output
Spindle stop
Encoder selection
Spindle command selection Spindle
selection
Spindle enable
SWS
SWS
SWS
SWS
Spindle rotation speed input
(Note) Refer to the PLC Interface Manual for details on each signal.
10. Spindle Functions 10.6 Multiple Spindle Control
159
Relation with other functions
(1) Spindle clamp speed setting (G92)
This is valid only on the spindle selected with the spindle selection signal (SWS). The spindle not selected with the spindle selection signal (SWS) maintains the speed at which it was rotating at before being canceled. (The spindle clamp speed is maintained with the G92 command.)
(2) Constant surface speed control Constant surface speed control can be applied on all spindles. The spindle rotation speed is automatically controlled during constant surface speed control, so when machining with constant surface speed, the spindle selection signal (SWS) for that spindle must be left ON. The spindle not selected with the spindle selection signal (SWS) maintains the speed at which it was rotating at before being canceled.
(3) Thread cutting/synchronous feed The threads are cut with the spindle selected with the spindle selection signal (SWS). The encoder feedback selected with the encoder selection signal is used.
(4) Synchronous tap The synchronous tap spindle is selected with the spindle selection signal (SWS). Select the synchronous tap spindle before issuing the synchronous tap command. Do not change the synchronous tap spindle selection signal during the synchronous tapping mode. If a C axis mode command is issued to the synchronous tap spindle, the «M01 operation error 1026» will occur. When the C axis command is canceled, the error will be canceled and machining will resume. If a polygon machining command is issued to the synchronous tap spindle, the «M01 operation error 1026» will occur. When the polygon machining command is canceled, the error will be canceled and machining will resume.
(5) Asynchronous tap The asynchronous tap spindle is selected with the spindle selection signal (SWS). Select the asynchronous tap spindle before issuing the tap command. Input a calculation request to change the asynchronous tap spindle selection. Do not change the asynchronous tap spindle selection signal during the asynchronous tapping mode.
(6) Tap return The tap return spindle is selected with the spindle selection signal (SWS). Select the spindle for which the tap cycle execution is stopped before turning the tap return signal ON. If tap return is executed when a different spindle is selected, the «M01 operation error 1032» will occur. Do not change the spindle selection signal during tap return.
Restrictions
(1) The S manual value command is invalid when multiple spindle control II is valid.
(2) Setup parameter «#1199 Sselect» is invalid when multiple spindle control II is valid.
(3) The spindle control mode changeover G code cannot be used when multiple spindle control II is valid. A program error (P34) will occur.
(4) The «S1=» and «S2=» commands are invalid when multiple spindle control II is valid. A program error (P33) will occur.
(5) The spindle gear shift command output signal (GR1/GR2) is not output when multiple spindle control II is valid.
11. Tool Functions (T command) 11.1 Tool Functions (T8-digit BCD)
160
11. Tool Functions (T command) 11.1 Tool Functions (T8-digit BCD)
Function and purpose
The tool functions are also known simply as T functions and they assign the tool numbers and tool offset number. They are designated with a 8-digit number following the address T, and one set can be commanded in one block. The output signal is an 8-digit BCD signal and start signal. If the T function is designated in the same block as a movement command, the commands may be executed in either of the following two orders. The machine specifications determine which sequence applies.
(1) The T function is executed after the movement command.
(2) The T function is executed simultaneously with the movement command.
Processing and completion sequences are required for all T commands.
12. Tool Compensation Functions 12.1 Tool Compensation
161
12. Tool Compensation Functions 12.1 Tool Compensation
Function and purpose
The basic tool compensation function includes the tool length compensation and tool radius compensation. Each compensation amount is designated with the tool compensation No. Each compensation amount is input from the setting and display unit or the program.
(Side view)
Reference position
Tool length Tool length compensation
Right compensation
Left compensation
(Plane view)
Tool radius compensation
12. Tool Compensation Functions 12.1 Tool Compensation
162
Tool compensation memory
There are two types of tool compensation memories for setting and selecting the tool compensation amount. (The type used is determined by the machine maker specifications.) The compensation amount settings are preset with the setting and display unit. Type 1 is selected when parameter «#1037 cmdtyp» is set to «1», and type 2 is selected when set to «2».
Type of tool compensation
memory
Classification of length compensation, radius compensation
Classification of shape compensation, wear compensation
Type 1 Not applied Not applied Type 2 Applied Applied
Reference
Reference tool
Shape
Tool length compensation
Wear amount
Shape
Tool radius compensation
Wear amount
12. Tool Compensation Functions 12.1 Tool Compensation
163
Type 1
One compensation amount corresponds to one compensation No. as shown on the right. Thus, these can be used commonly regardless of the tool length compensation amount, tool radius compensation amount, shape compensation amount and wear compensation amount. (D1) = a1 , (H1) = a1 (D2) = a2 , (H2) = a2 : : (Dn) = an , (Hn) = an
Compensation No. Compensation amount
1 a1 2 a2 3 a3 n an
Type 2
The shape compensation amount related to the tool length, wear compensation amount, shape compensation related to the tool radius and the wear compensation amount can be set independently for one compensation No. as shown below. The tool length compensation amount is set with H, and the tool radius compensation amount with D. (H1) = b1 + c1, (D1) = d1 + e1 (H2) = b2 + c2, (D2) = d2 + e2 : : (Hn) = bn + cn, (Dn) = dn + en
Tool length (H) Tool radius (D)/ (Position compensation) Compe
nsation No.
Shape compensation
amount
Wear compensation
amount
Shape compensation
amount
Wear compensation
amount 1 b1 c1 d1 e1 2 b2 c2 d2 e2 3 b3 c3 d3 e3 n bn cn dn en
CAUTION
If the tool compensation amount is changed during automatic operation (including during single block stop), it will be validated from the next block or blocks onwards.
12. Tool Compensation Functions 12.1 Tool Compensation
164
Tool compensation No. (H/D)
This address designates the tool compensation No.
(1) H is used for the tool length compensation, and D is used for the tool position offset and tool
radius compensation. (2) The tool compensation No. that is designated once does not change until a new H or D is
designated. (3) The compensation No. can be commanded once in each block. (If two or more Nos. are
commanded, the latter one will be valid.) (4) The No. of compensation sets that can be used will differ according to the machine. For 40 sets: Designate with the H01 to H40 (D01 to D40) numbers. (5) If a value larger than this is set, the program error (P170) will occur. (6) The setting value ranges are as follows for each No. The compensation amount for each compensation No. is preset with the setting and display
unit. Shape compensation amount Wear compensation amount Setting Metric system Inch system Metric system Inch system
#1003=B 99999.999 (mm)
9999.9999 (inch)
99999.999 (mm)
9999.9999 (inch)
#1003=C 99999.9999 (mm)
9999.99999 (inch)
99999.9999 (mm)
9999.99999 (inch)
#1003=D 99999.99999 (mm)
9999.999999 (inch)
99999.99999 (mm)
9999.999999 (inch)
#1003=E 99999.999999 (mm)
9999.9999999 (inch)
99999.999999 (mm)
9999.9999999 (inch)
12. Tool Compensation Functions 12.2 Tool Length Compensation/Cancel; G43, G44/G49
165
12.2 Tool Length Compensation/Cancel; G43, G44/G49
Function and purpose
The end position of the movement command can be compensation by the preset amount when this command is used. A continuity can be applied to the program by setting the actual deviation from the tool length value decided during programming as the compensation amount using this function.
Command format
When tool length compensation is + When tool length compensation is G43 Zz Hh ; :
Tool length compensation (+) start
G44 Zz Hh ; :
Tool length compensation () start
G49 Zz ; Tool length compensation cancel
G49 Zz ; Tool length compensation cancel
Detailed description
(1) Tool length compensation movement amount
The movement amount is calculated with the following expressions when the G43 or G44 tool length compensation command or G49 tool length compensation cancel command is issued.
Z axis move-
ment amount
G43 Zz Hn1 ; z + (lh1) Compensation in + direction by tool compensation amount G44 Zz Hh1 ; z — (lh1) Compensation in — direction by tool compensation amount G49 Zz ; z — (+) (lh1) Compensation amount cancel (Note) lh1 : Compensation amount for compensation No. h1
Regardless of the absolute value command or incremental value command, the actual end point will be the point compensated by the compensation amount designated for the programmed movement command end point coordinate value. The G49 (tool length compensation cancel) mode is entered when the power is turned ON or when M02 has been executed. (Example 1) For absolute value command
H01 = -100000 N1 G28 Z0 T01 M06 ; N2 G90 G92 Z0 ; N3 G43 Z5000 H01 ; N4 G01 Z-50000 F500 ;
(Example 2) For incremental value command
H01 = -100000 N1 G28 Z0 T01 M06 ; N2 G91 G92 Z0 ; N3 G43 Z5000 H01 ;
N4 G01 Z-55000 F500 ;
Tool length compensation H01=-100.
W or
kp ie
ce
R
+5.00
0 W
-50.000
12. Tool Compensation Functions 12.2 Tool Length Compensation/Cancel; G43, G44/G49
166
(2) Compensation No.
(a) The compensation amount differs according to the compensation type. Type 1
G43 Hh1 ; When the above is commanded, the compensation amount lh1 commanded with compensation No. h1 will be applied commonly regardless of the tool length compensation amount, tool radius compensation amount, shape compensation amount or wear compensation amount.
Table
lh1
R
Workpiece
Type 2
G43 Hh1 ; When the above is commanded, the compensation amount lh1 commanded with compensation No. h1 will be as follows. lh1: Shape compensation + wear compensation amount
Table
R
Workpiece
Shape compensation amountlh1
Wear compensation amount
(b) The valid range of the compensation No. will differ according to the specifications (No. of compensation sets).
(c) If the commanded compensation No. exceeds the specification range, the program error (P170) will occur.
(d) Tool length cancel will be applied when H0 is designated. (e) The compensation No. commanded in the same block as G43 or G44 will be valid for the
following modals.
(Example 3) G43 Zz1 Hh1 ; ………..Tool length compensation is executed with h1. : G45 Xx1 Yy1 Hh6 ; : G49 Zz2 ; ……………….The tool length compensation is canceled. : G43 Zz2 ; ……………….Tool length compensation is executed again with h1. :
(f) If G43 is commanded in the G43 modal, a compensation of the difference between the
compensation No. data will be executed.
(Example 4) G43 Zz1 Hh1 ; ……….. Becomes the z1 + (lh1) movement. : G43 Zz2 Hh2 ; ……….. Becomes the z2 + (lh2 — lh1) movement. :
The same applies for the G44 command in the G44 modal.
12. Tool Compensation Functions 12.2 Tool Length Compensation/Cancel; G43, G44/G49
167
(3) Axis valid for tool length compensation
(a) When parameter «#1080 Dril_Z» is set to «1», the tool length compensation is always applied on the Z axis.
(b) When parameter «#1080 Dril_Z» is set to «0», the axis will depend on the axis address commanded in the same block as G43. The order of priority is shown below.
Zp > Yp > Xp
(Example 5) G43 Xx1 Hh1 ; …………….+ compensation to X axis : G49 Xx2 ; : G44 Yy1 Hh2 ; …………….-compensation to Y axis : G49 Yy2 ; : G43 1 Hh3 ;……………..+ compensation to additional axis : G49 1 ; : G43 Xx3 Yy3 Zz3 ; ………Compensation is applied on Z axis : G49 ;
The handling of the additional axis will follow the parameters «#1029 to 1031 aux_I, J and K» settings. If the tool length compensation is commanded for the rotary axis, set the rotary axis name for one of the parallel axes.
(c) If H (compensation No.) is not designated in the same block as G43, the Z axis will be
valid.
(Example 6) G43 Hh1 ; …………………….Compensation and cancel to X axis : 49 ;
(4) Movement during other commands in tool length compensation modal
(a) If reference position return is executed with G28 and manual operation, the tool length compensation will be canceled when the reference position return is completed.
(Example 7)
G43 Zz1 Hh1 ; : G28 Zz2 ; ……………………Canceled when reference position is reached. : G43 Zz2 Hh2 ; (Same as G49) : G49 G28 Zz2 ; …………….After the Z axis is canceled, reference position
return is executed. (b) The movement is commanded to the G53 machine coordinate system, the axis will move
to the machine position when the tool compensation amount is canceled. When the G54 to G59 workpiece coordinate system is returned to, the position returned to will be the coordinates shifted by the tool compensation amount.
12. Tool Compensation Functions 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G49
168
12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G49
Function and purpose
(1) Changes in the tool length compensation in the tool axis direction and compensation amount
The tool length can be compensated in the tool axis direction even when the rotation axis rotates and the tool axis direction becomes other than the Z axis direction. By using this function, and setting the deviation between the tool length amount set in the program and the actual tool length as the compensation amount, a more flexible program can be created. This is especially valid for programs in which many rotation axis movement commands are present. The tool length compensation amount in the tool axis direction can be changed by rotating the manual pulse generator when the tool length compensation amount in the tool axis direction is being changed during the tool length compensation in the tool axis direction mode.
(2) Machine configuration
The compensation using the tool length compensation in the tool axis direction function is applied to the direction of the tool tip axis (rotary axis). As for the axes that determine the compensation direction, a combination of the C axis (spindle) for Z axis rotation and the A axis for X axis rotation or B axis for Y axis rotation is designated using a parameter.
Rotation center
Tool
Axis direction (compensation direction)
Workpiece
Axis C
Axis A or B
Y
Z
X
A B
C
Rotation center
Tool
Axis direction (compensation direction)
Axis A
Axis B
Workpiece
Axis A or B Axis B or C Axis A or B
Command format
G43.1 X__ Y__ Z__ H__ ; G49 X__ Y__ Z__ ;
Tool length compensation in the tool axis direction Tool length compensation cancel
X, Y, Z H
: Movement data : Tool length compensation No.
(If the compensation No. exceeds the specification range, a program error (P170) will occur.
12. Tool Compensation Functions 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G49
169
Detailed description
(1) G43, G44 and G43.1 are all G codes in the same group. Therefore, it is not possible to
designate more than one of these commands simultaneously for compensation. G49 is used to cancel the G43, G44 and G43.1 commands.
(2) If the G43.1 command is designated when the option for the tool length compensation in the
tool axis direction is not provided, the program error (P930) will occur. (3) If reference position has not been completed for any of the X, Y, Z, A or B and C axes in the
G43.1 block, the program error (P430) will occur. However, the error does not apply to the following cases. — When mechanical axes have been selected: The error does not apply to the A, B and C axes. — When «1» has been set for the «#2031 noref» zero point return parameter: The error does not apply to the axis for which «noref» is set to «1» because it is considered that the reference position return of the axis has already completed.
Changing the amount of tool length compensation in the tool axis direction
(1) When the following conditions have been met, the handle movement amount is added to the
tool length compensation amount in the tool axis direction by rotating the manual pulse generator. When the operation mode is MDI, memory or tape operation mode and the state is «during single block stop», «during feed hold» or «during cutting feed movement». Note that compensation amount cannot be changed during error or warning. During tool length compensation in the tool axis direction (G43.1). In the tool length compensation amount in the tool axis direction changing mode (YC92/1). In the tool handle feed & interruption mode (YC5E/1). The 3rd axis (tool axis) is selected for the handle selection axis.
(2) The change amount is canceled when the compensation No. is changed. (Note 1) The coordinate value in the tool length compensation amount in the tool axis direction
change mode operates in the same manner as that when the manual ABS is ON, regardless of manual ABS switch (YC28) or base axis specification parameter «#1061 intabs».
(Note 2) If compensation amount is changed during continuous operation, single block stop, or feed hold, the compensation amount will be effective immediately in the next block.
(Example) When changing compensation amount during continuous operation.
Changed compensation amount
Compensation amount before change
Path after compensation
Program path
Workpiece
12. Tool Compensation Functions 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G49
170
(Example) When changing compensation amount during single block stop.
Changed compensation amount
Compensation amount before change
Path after compensation
Program path
Workpiece
Single block stop
Changed compensation amount
(Note 3) When changing compensation amount, the compensation amount corresponding to the actual compensation No. will be changed. However, when executing the NC reset or tool length compensation in the direction of tool axis cancel (G49), the compensation amount will be returned to the original.
Tool length compensation in the tool axis direction vector
The vectors representing the tool length compensation in the tool axis direction are as follows. (1) When the A and C axes are set as the rotary axes:
Vx = L sin (A) sin (C) Vy = -L sin (A) cos (C) Vz = L cos (A)
(2) When the B and C axes are set as the rotary axes:
Vx = L sin (B) cos (C) Vy = L sin (B) sin (C) Vz = L cos (B)
Vx, Vy, Vz : Tool length compensation in the tool axis direction vectors for X, Y and Z axes L : Tool length compensation amount (1h) A, B, C : Rotation angle (machine coordinate position) of A, B and C axes
Path after tool length compensation in the tool axis direction
Program path G43.1 command
G44 command
12. Tool Compensation Functions 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G49
171
(3) Rotary axis angle command
The value used for the angle of the rotary axis (tool tip axis) differs according to the type of rotary axis involved.
When servo axes are used: The machine coordinate position is used for the rotation angles of the A, B and C axes.
When mechanical axes are used: Instead of the machine coordinate position of the axes, the values read out from the R registers (R2628 to R2631) are used for the rotation angles of the A, B and C axes.
Compensation amount resetting
Tool length compensation in the tool axis direction is cleared in the following cases. (1) When manual reference position return is completed. (2) When reset 1, reset 2 or reset & rewind has been executed. (3) When the G49 command has been designated. (4) When the compensation No. 0 command has been executed. (5) When NC reset has been executed with «1» set for the basic system parameter «#1151 rstint». (6) When the G53 command is designated while the compensation status is still established, the
compensation is temporarily canceled, and the tool moves to the machine position designated by G53.
12. Tool Compensation Functions 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G49
172
Example of program
(1) Example of arc machining
Shown below is an example of a program for linear arc arc linear machining using the B and C rotary axes on the ZX plane.
X axis
Tool length compensation amount
Example of program
Tool with no compensation
N09
N10
Path after compensation
Programmed path
N07
Z axis
N12
N11
N08
Machining program N01 G91 G28 X0 Y0 Z0 ; Compensation amount H01 = 50 mm N02 G28 B0 C0 ; N03 G90 G54 G00 X400. Y0 ; N04 Z-150. ; N05 B90. ; B axis: 90 degrees N06 G18 ; N07 G43.1 X250. H01 ; Tool length compensation in the tool axis
direction ON N08 G01 Z0 F200 ; N09 G02 X0 Z250. I-250. K0 B0 ; Top right arc, B axis: 0 degrees N10 G02 X-250. Z0 I0 K-250. B-90. ; Bottom right arc, B axis: -90 degrees N11 G01 Z-150. ; N12 G00 G44 X-400. ; Tool length compensation in the tool axis
direction OFF N13 G91 G28 B0 C0 ; N14 G28 X0 Y0 Z0 ; N15 M02 ;
X axis
Tool length compensation amount
(Reference) Example of tool length compensation (G43)
N09
N10
Path after compensation
Programmed path
N07
Z axis
N12
N11
N08
12. Tool Compensation Functions 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G49
173
Relation with other functions
(1) Relation with 3-dimensional coordinate conversion
(a) A program error (P931) will occur if 3-dimensional coordinate conversion is carried out during tool length compensation in the tool axis direction.
(b) A program error (P921) will occur if the tool length is compensated in the tool axis direction during 3-dimensional coordinate conversion.
(c) A program error (P923) will occur if the tool length compensation in the tool axis direction is commanded in the same block as the 3-dimensional coordinate conversion.
(2) Relation with automatic reference position return
(a) A program error (P931) will occur if a command from G27 to G30 is issued during tool length compensation in the tool axis direction.
(3) Relation with manual reference position return
(a) Reference position return for the orthogonal axis Tool length compensation in the tool axis direction will be canceled, as well as the dog-type reference position return and the high-speed reference position return.
N1G90G00G54X0Y0Z0 ; Positioning to the workpiece origin N2G00A45. ; Rotating the rotary axis by 45 N3G43.1H1 ; Tool length compensation in the tool axis
direction ON N4G19G03Y-5.858Z-14.142J14.142K-14.142A90.; Circular cutting *Manual dog-type reference position return N5G00Y0. ; N6Z0. :
:
Manual dog-type reference position return
Z
Y M
N2
N1
N4
N3 W
45
N5G00Y0. ; Positioning to the position where tool length
compensation in the tool axis direction was canceled.
N6Z0. Positioning to the position where tool length
compensation in the tool axis direction was canceled.
: :
Z
Y M
W
N6
N5
12. Tool Compensation Functions 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G49
174
(b) Reference position return for the rotary axis
Tool length compensation in the tool axis direction will be canceled, as well as the dog-type reference position return and the high-speed reference position return.
N1G90G00G54X0Y0Z0 ; Positioning to workpiece origin N2G00A45. ; Rotating the rotary axis by 45 N3G43.1H1 ; Tool length compensation in the tool
axis direction ON N4G19G03Y-5.858Z-14.142J14.142K-14.142A90.; Circular cutting *Manual dog-type reference position return N5G00Y0. ; N6Z0. : :
Z
Y M
N2 45
N3W
N3
N4
90
Manual dog-type reference position return
N5
N6
Z
M Y
W N5G00Y0. ; Positioning to the position where tool
length compensation in the tool axis direction was canceled.
N6Z0. ; Positioning to the position where tool
length compensation in the tool axis direction was canceled.
: :
(4) Relation with graphic check
(a) Graphic check draws a path after compensation.
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
175
12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
Function and purpose
This function compensates the radius of the tool. The compensation can be done in the random vector direction by the radius amount of the tool selected with the G command (G38 to G42) and the D command.
Command format
G40X__Y__ ; : Tool radius compensation cancel G41X__Y__ ; : Tool radius compensation (left) G42X__Y__ ; : Tool radius compensation (right) G38I__J__ ; : Change or hold of compensation vector G39X__Y__ ; : Corner changeover
Can be commanded only during the radius compensation mode.
Detailed description
The No. of compensation sets will differ according to the machine model. (The No. of sets is the total of the tool length offset, tool position offset and tool radius compensation sets.) The H command is ignored during the tool radius compensation, and only the D command is valid. The compensation will be executed within the plane designated with the plane selection G code or axis address 2 axis, and axes other than those included in the designated plane and the axes parallel to the designated plane will not be affected. Refer to the section on plane selection for details on selecting the plane with the G code.
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
176
12.4.1 Tool radius Compensation Operation
Tool radius compensation cancel mode
The tool radius compensation cancel mode is established by any of the following conditions.
(1) After the power has been switched on (2) After the reset button on the setting and display unit has been pressed (3) After the M02 or M30 command with reset function has been executed (4) After the tool radius compensation cancel command (G40) has been executed
The offset vectors are zero in the compensation cancel mode, and the tool nose point path coincides with the programmed path. Programs including tool radius compensation must be terminated in the compensation cancel mode.
Tool radius compensation start (start-up)
Tool radius compensation starts when all the following conditions are met in the compensation cancel mode.
(1) The movement command is issued after G41 or G42. (2) The tool radius compensation offset No. is 0 < D max. offset No. (3) The movement command of positioning (G00) or linear interpolation (G01) is issued.
At the start of compensation, the operation is executed after at least three movement command blocks (if three movement command blocks are not available, after five movement command blocks) have been read regardless of the continuous operation or single block operation. During compensation, 5 blocks are pre-read and the compensation is arithmetically processed. Control mode transition diagram
Machining program Pre-read buffer Execution block
T__; S__;
T__; S__;
G00_;
G00_; G41_; G01_; G02_;
G02_; G01_; G41_;
T____; S____; G00____; G41____; G01____; G02____;
G01_; G02_;
Start of pre-reading 5 blocks
There are two ways of starting the compensation operation: type A and type B. The type can be selected with bit 2 of parameter «#1229 set 01». This type is used in common with the compensation cancel type. In the following explanatory figure, «S» denotes the single block stop point.
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
177
Start of movement for tool radius compensation
(1) For inner side of corner
r = Compensation amount
Start point
G42
s s
G42
r
Program path
Tool center path
Program path
Tool center path
Center of circular
Linear Linear Linear Circular
Start point
(2) For outer side of corner (obtuse angle) [900<180]
r = Compensation amount
Tool center path
Program path
Start point Center of circular
Linear Linear(Type A)
G41
s
G41
r
s
G41
r r
s
r r
s
Start point
Tool center path
Program path
Tool center path
Center of circular Start point
Point of intersection
G41
Tool center path
Program path
Linear Circular(Type A)
Linear Linear(Type B)
Start point
Linear Circular(Type B)
Point of intersection
Program path
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
178
(3) For outer side of corner (obtuse angle) [0<90]
G41
r
s
Start point
Tool center path
Program path
r
s
Start point
G41
Tool center path
Program path
Center of circular
Linear Circular(Type A)
r
r
s
Tool center path
Program path
Start point
G41
Linear Linear(Type B)
r
r
s
G41
Start point
Center of circular
Tool center path
Program path
Linear Circular(Type B)
Linear Linear(Type A)
(Note) If there is axis movement command in the same block as G41 or G42, compensation is
performed perpendicularly to the next block’s direction.
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
179
Operation in compensation mode
Relative to the program path (G00, G01, G02, G03), the tool center path is found from the straight line/circular arc to make compensation. Even if the same compensation command (G41, G42) is issued in the compensation mode, the command will be ignored. When 4 or more blocks not accompanying movement are commanded continuously in the compensation mode, overcutting or undercutting will result. When the M00 command has been issued during tool radius compensation, pre-reading is prohibited.
(1) Machining an outer wall
Tool center path
Program path
Point of intersection
Linear Linear (90<180)
s
Linear Linear (0<<90)
r
r
s
Tool center path
Program path
Center of circular
r
r
s
Linear Circular (0<<90)
s
r
r
Linear Circular (90180)
Tool center path
Program path
Tool center path
Program path
Center of circular
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
180
Tool center path
Point of intersection
Center of circular
Circular Linear (0<<90)
r
r
s
Circular Linear (90<180)
r r
s
Program path
Center of circular
Program path
Tool center path
Tool center path
Program path
Point of intersection
Center of circular
Circular Circular (90<180)
r r
s
Circular Circular (0<<90)
r r
s
Center of circular
Center of circular Center of circular
Tool center path
Program path
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
181
(2) Machining an inner wall
Tool center path
Program path
Point of intersection
Linear Linear (Obtuse angle)
r s
Linear Linear (Acute angle)
r
r s
r
Linear Circular (Obtuse angle)
s
r
r
Linear Circular (Acute angle)
s
r
Circular Linear (Acute angle)
s
r
Circular Linear (Obtuse angle)
s
Tool center path
Program path
Tool center path
Program path
Point of intersection
Center of circular
Tool center path
Program path
Point of intersection
Center of circular
Tool center path
Program path
Center of circular
Point of intersection Tool center path
Program path
Center of circular
Point of intersection
Tool center path
Program path
Point of intersection
Center of circular
Circular Linear (Obtuse angle)
r
s
Center of circular
Circular Linear (Acute angle)
r
s
Center of circular
Center of
Tool center path Point of
intersection
Program path
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
182
(3) When the arc end point is not on the arc
For spiral arc ……………………….. A spiral arc will be interpolated from the start to end point of the arc.
For normal arc command………. If the error after compensation is within parameter «#1084 RadErr», the area from the arc start point to the end point is interpolated as a spiral arc.
Center of circular
End point of circular
Program path
Hypothetical circle
r
r s
R
Tool center path
(4) When the inner intersection point does not exist In an instance such as that shown in the figure below, the intersection point of arcs A and B may cease to exist due to the offset amount. In such cases, program error (P152) appears and the tool stops at the end point of the previous block.
Program error stop
Line intersecting circulars A, B
Tool center path
Program path
Center of circular A
r
r
A B
Tool radius compensation cancel
If either of the following conditions is met in the tool radius compensation mode, the compensation will be canceled. However, the movement command must be a command which is not a circular command. If the compensation is canceled by a circular command, program error (P151) results.
(1) The G40 command has been executed. (2) The D00 tool number has been executed.
The cancel mode is established once the compensation cancel command has been read, 5-block pre-reading is suspended and 1-block pre-reading is made operational.
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
183
Tool radius compensation cancel operation
(1) For inner side of corner
r = Compensation amount
Tool center path
Program path
End point
Linear Linear
s
G40
Circular Linear
r
s
G40
Center of circular End point
Tool center path
Program path
(2) For outer side of corner (obtuse angle)
r = Compensation amount
Tool center path
Program path
End point Center of circular
Linear Linear (Type A)
s
G40
Circular Linear (Type A)
r
s
Linear Linear (Type B)
r
s
r
Circular Linear (Type B)
r
s
r
G40
End point Program path
Tool center path
Point of intersection
Program path
Tool center path
Center of circular End point
G40
Tool center path
Program path
End point
G40
Point of intersection
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
184
(3) For outer side of corner (acute angle)
Tool center path
End point
Program path
Linear Linear (Type A)
r
s
G40
Circular Linear (Type A)
s
G40
r
Tool center path
Program path
End point
Center of circular
Linear Linear (Type B)
r
s
G40
r
Tool center path
End point
Program path
Circular Linear (Type B)
r
s
G40
r
Tool center path
Program path
Center of circular
End point
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
185
12.4.2 Other Commands and Operations during Tool Radius Compensation
Insertion of corner arc
An arc that uses the compensation amount as the radius is inserted without calculating the point of intersection at the workpiece corner when G39 (corner arc) is commanded.
Inserted circular Tool center path
r = Compensation amount
Program path
(With G39 command)
For outer side compensation
Point of intersection
(No G39 command)
s
s
For inner side compensation
Inserted circular
Tool center path
r = Compensation amount
Program path
(With G39 command)
Point of intersection
(No G39 command)
Tool center path
Program path
N1 G28X0Y0 ; N2 G91G01G42X20.Y20.D1F100 ; N3 G39X40. ; N4 G39Y40. ; N5 G39X-40. ; N6 Y-40. ; N7 G40X-20.Y-20. ; N8 M02 ;
N2
N1
D1=5.000
N3
N4
N5
N6
N7
Y
X
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
186
Changing and holding of compensation vector
The compensation vector can be changed or held during tool radius compensation by using the G38 command.
(1) Holding of vector: When G38 is commanded in a block having a movement command, the
point of intersection will not be calculated at the program end point, and instead the vector of the previous block will be held.
G38 Xx Yy ; This can be used for pick feed, etc.
(1) Holding the inside compensation vector (2) Holding the outside compensation acute angle
Program path
N11G1Xx11; N12G38Xx12Yy12; N13G40Xx13;
Tool center path
r1: Vector at N11-N12 block intersection calculation
N11
N12
N13 r1
r1
Program path N11G1Xx11Yy11; N12G38Xx12Yy12; N13G40Xx13;
Tool center path
N11 N12
N13
r1
r1
r1: Vector at N11-N12 block intersection calculation
(3) Holding the outside compensation obtuse angle
r1: Vector at N11-N12 block intersection calculation
Program path N11G1Xx11Yy11; N12G38Xx12Yy12; N13G40Xx13;
Tool center path
N11 N12
N13
r1
r1
(2) Changing of vector: A new compensation vector direction can be commanded with I, J and K,
and a new offset amount with D. (These can be commanded in the same block as the movement
command.) G38 Ii Jj Dd ; (I, J and K will differ according to the selected plane.)
Program path
N11G1Xx11; N12Yy12; N13G38Xx13IiJjDd; N14G40Xx14Yy14;
Tool center path
The compensation amount d vector is created in the commanded i and j vector direction.
N13
N12
N11
i
j
N14
d d
(Note) If G38 is commanded in the same block as the circular block (G02/G03) I and J commands, I and J will be handled as the G38 vector, and an error will occur.
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
187
Changing the compensation direction during tool radius compensation
The compensation direction is determined by the tool radius compensation commands (G41, G42) and compensation amount sign.
Compensation amount sign
G code + —
G41 Left-hand compensation Right-hand compensation
G42 Right-hand compensation Left-hand compensation The compensation direction can be changed by changing the compensation command in the compensation mode without the compensation having to be first canceled. However, no change is possible in the compensation start block and the following block. Refer to section «12.4.5 General precautions for tool radius compensation» for the movement when the symbol is changed.
Point of intersection
Tool center path
Program path
r
G41
r
Linear Linear
G41 G42
r
r
If there is no point of intersection when the compensation direction is changed.
Linear Circular
Tool center path
Program path
r
G41
r
G41 G42 G41G42
r
r
r
r
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
188
Tool center path
Program path
Circular center
Circular center G42 G41 G41
G41
G41
G42
Circular Circular
Linear return
Tool center path Program path
G41
G42 r
Tool center path
Program path
Uncut section
Arc exceeding 360 due to compensation
G41
G42
G42
In the case below, it is possible that the arc may exceed 360 a. With offset direction selection based on
G41/G42 b. I, J, K was commanded in G40. In cases like this the tool center path will pass through a section where the arc is doubled due to the compensation and a section will be left uncut.
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
189
Command for eliminating compensation vectors temporarily
When the following command is issued in the compensation mode, the offset vectors are temporarily eliminated and a return is then made automatically to the compensation mode. In this case, the compensation is not canceled, and the tool goes directly from the intersection point vector to the point without vectors or, in other words, to the programmed command point. When a return is made to the compensation mode, it goes directly to the intersection point.
(1) Reference position return command
Intermediate point
N6N5
S
S
S
N8 N7
(G41) ~ N5 G91 G01 X60. Y30. ; N6 G28 X50. Y-40. ; N7 X30. Y-60. ; N8 X70. Y40. ;
~
Temporarily no compensation vectors at intermediate point.
(Reference position when there is no intermediate point)
(2) G33 thread cutting command
Tool nose radius compensation does not apply to the G33 block.
Point of intersection Tool center path
Program path
r (G41)
G33
(3) The compensation vector will be eliminated temporarily with the G53 command (basic machine coordinate system selection).
(Note 1) The compensation vectors do not change with the coordinate system setting (G92)
command.
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
190
Blocks without movement and pre-read inhibit M command
The following blocks are known as blocks without movement.
a. M03 ; ……………………………M command b. S12 ; …………………………….S command c. T45 ; …………………………….T command d. G04 X500 ; ……………………Dwell e. G22 X200. Y150. Z100 ; ….Machining inhibit region setting f. G10 L10 P01 R50 ; …………Offset amount setting g. G92 X600. Y400. Z500. ; …Coordinate system setting h. (G17) Z40. ; ………………..Movement but not on offset plane i. G90 ; …………………………….G code only j. G91 X0 ; ……………………….Zero movement amount ….. Movement amount is zero
No movement
M00, M01, M02 and M30 are handled as pre-read inhibit M codes. (1) When command is assigned at start of the compensation
Perpendicular compensation will be applied on the next movement block.
N1
N2
N3
N4
N1 X30. Y60. ;
N2 G41 D10 ;
N3 X20. Y-50. ;
N4 X50. Y-20. ;
Block without movement
If four or more blocks containing no move command continue or if there is a pre-read inhibit M code, no compensation vector is generated.
N1
N2, 3, 4, 5, 6
N7
N8
N1 X30. Y60. ; N2 G41 D10 ; N3 G4 X1000 ; N4 F100 ; N5 S500 ; N6 M3 ; N7 X20. Y-50. ; N8 X50. Y-20. ;
Block without movement
Point of intersection
Point of intersection N1
N2 N5
N6
N7
N1 G41 X30. Y60. D10 ; N2 G4 X1000 ; N3 F100 ; N4 S500 ; N5 M3 ; N6 X20. Y-50. ; N7 X50. Y-20. ;
Block without movement
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
191
(2) When command is assigned in the compensation mode
When 4 or more blocks without movement follow in succession in the compensation mode or when there is no pre-read inhibit M code, the intersection point vectors will be created as usual.
N8 N6
N7
N6
N8 N6 G91 X100. Y200. ;
N7 G04 X P1000 ;
N8 X200. ; Block without movement
Block N7 is executed here.
When 4 or more blocks without movement follow in succession or if there is a pre-read inhibit M code, the offset vectors are created perpendicularly at the end point of the previous block.
N11
N6 N7 N10
N6
N11 N6 X100. Y200. ;
N7 G4 X1000 ;
N8 F100 ;
N9 S500 ;
N10 M4 ;
N11 W100. ;
In this case, a cut results.
Block without movement
(3) When commanded together with compensation cancel
N6 X100. Y200. ; N7 G40 M5 ; N8 X100. Y50. ;
N6
N7
N8
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
192
When I, J, K are commanded in G40
(1) If the final movement command block in the four blocks before the G40 block is the G41 or
G42 mode, it will be assumed that the movement is commanded in the vector I, J or K direction from the end point of the final movement command. After interpolating between the hypothetical tool center path and point of intersection, it will be canceled. The compensation direction will not change.
Tool center path
Program path
Hypothetical tool center path
N1 (G41) G1X_ ; N2 G40XaYbIiJj;
r N1
(i,j) N2 A
(a,b)
r G41
In this case, the point of intersection will always be obtained, regardless of the compensation direction, even when the commanded vector is incorrect as shown below.
Tool center path
Program path
Hypothetical tool center path
r N1
(i,j)
N2
A
(a,b)
r
G41 When the I and j symbols in the above program example are incorrect
If the compensation vector obtained with point of intersection calculation is extremely large, a perpendicular vector will be created in the block before G40.
Tool center path
Program path
Hypothetical tool center path r
G40
(i,j)
A
(a,b)
r G41
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
193
(2) If the arc is 360 or more due to the details of I, J and K at G40 after the arc command, an
uncut section will occur.
Tool center path Program path
Uncut section
N1 (G42,G91) G01X200. ; N2 G02 J150. ; N3 G40 G1X150. Y-150. I-100. J100. ;
r
N1
(i,j)
N2
r G42
r
G40 N3
Corner movement
When a multiple number of offset vectors are created at the joints between movement command blocks, the tool will move in a straight line between those vectors. This action is called corner movement. When the vectors do not coincide, the tool moves in order to machine the corner although this movement is part and parcel of the joint block. Consequently, operation in the single block mode will execute the previous block + corner movement as a single block and the remaining joining movement + following block will be executed as a single block in the following operation.
Tool center path
Program path
This movement and feedrate fall under block N2.
Stop point with single block
Center of circular r
N1
N2
r
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
194
12.4.3 G41/G42 Commands and I, J, K Designation
Function and purpose
The compensation direction can be intentionally changed by issuing the G41/G42 command and I, J, K in the same block.
Command format
G17 (XY plane) G41/G42 X__ Y__ I__ J__ ; G18 (ZX plane) G41/G42 X__ Z__ I__ K__ ; G19 (YZ plane) G41/G42 Y__ Z__ J__ K__ ;
Assign an linear command (G00, G01) in a movement mode.
I, J type vectors (G17 XY plane selection)
The new I, J type vector (G17 plane) created by this command is now described. (Similar descriptions apply to vector I, K for the G18 plane and to J, K for the G19 plane.) As shown in the figures, the vectors with a size equivalent to the offset amount are made to serve as the I, J type compensation vector perpendicularly to the direction designated by I, J without the intersection point of the programmed path being calculated. the I, J vector can be commanded even in the mode (G41/G42 mode in the block before) and even at the compensation start (G40 mode in the block before).
(1) When I, J is commanded at compensation start
Tool center path
Program path
(G40) N100 G91 G41 X100. Y100. I150. D1 ; N110 G04 X1000 ; N120 G01 F1000 ; N130 S500 ; N140 M03 ; N150 X150. ;
N150
N100
Y
X
N110 N120 N130 N140
D1
(2) When there are no movement commands at the compensation start.
(G40) N1 G41 I150. D1 ; N2 G91 X100. Y100. ; N3 X150. ;
N3
N2
Y
X
D1 N1
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
195
(3) When I, J has been commanded in the G41/G42 mode (G17 plane)
Tool path after interrupt
Program path Tool center path
(N120)
N100
Y
X
N120
(I,J)N110
D1
(2) (1)
(2)
(G17 G41 G91) N100 G41 G00X150. J50. ; N110 G02 I150. ; N120 G00 X150. ;
(1) I, J type vector (2) Intersection point calculation
type vector
(Reference) (a) G18 plane
(N120)
N100
Z
X
N120
(K,I) N110
(G18 G41 G91) N100 G41 G00 Z150. I50. ; N110 G02 K50. ; N120 G00 Z150. ;
(b) G19 plane
(N120)
N100
Z
Y
N120
(J,K) N110
(G19 G41 G91) N100 G41 G00 Y150. K50. ; N110 G02 J50. ; N120 G00 Y150. ;
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
196
(4) When I, J has been commanded in a block without movement
N1 G41 D1 G01 F1000 ; N2 G91 X100. Y100. ; N3 G41 I50. ; N4 X150. ; N5 G40 ;
N3
N2
D1 N1
N4
(I,J) N5
Direction of compensation vectors
(1) In G41 mode
Direction produced by rotating the direction commanded by I, J through 90 to the left from the forward direction of the Z axis (axis 3) as seen from the zero point (Example 1) With I100. (Example 2) With I-100.
Compensation vector direction
(100, 0) IJ direction
Compensation vector direction
(-100, 0 IJ direction)
(2) In G42 mode Direction produced by rotating the direction commanded by I, J through 90 to the right from the forward direction of the Z axis (axis 3) as seen from the zero point (Example 1) With I100. (Example 2) With I-100.
Compensation vector direction
(0, 100 IJ direction)
Compensation vector direction
(-100, 0) IJ direction
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
197
Selection of compensation modal
The G41 or G42 modal can be selected at any time.
N1 G28 X0 Y0 ; N2 G41 D1 F1000 ; N3 G01 G91 X100. Y100. ; N4 G42 X100. I100. J-100. D2 ; N5 X100. Y-100. ; N6 G40 ; N7 M02 ; %
N3
x
D1 N2
N6
(I,J)
N5
y
N4 D2
Compensation amount for compensation vectors
The offset amounts are determined by the offset number (modal) in the block with the I, J designation.
X N110
(I,J) A
Y N100
D1 D1
(G41 D1 G91) N100 G41 X150. I50. ; N110 X100. Y-100. ;
< Example 1>
Vector A is the offset amount entered in offset number modal D1 in the N200 block.
(G41 D1 G91) N200 G41 X150. I50. D2 ; N210 X100. Y-100. ;
X N210
(I,J)
B
Y N200
D2 D1
< Example 2>
Vector B is the offset amount entered in offset number modal D2 in the N200 block.
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
198
Precautions
(1) Issue the I, J type vector in a linear mode (G0, G1). If it is issued in an arc mode at the start of
compensation, program error (P151) will occur. An IJ designation in an arc mode functions as an arc center designation in the compensation mode.
(2) When the I, J type vector has been designated, it is not deleted (avoidance of interference) even if there is interference. Consequently, overcutting may arise in such a case.
N1 G28 X0Y0 ; N2 G42 D1 F1000 ; N3 G91 X100. ; N4 G42 X100. Y100. I10. ; N5 X100. Y-100. ; N6 G40 ; N7 M02 ;
Cut section
Y
X
N5
(I,J)
N4
N3
N2 N6
(3) The vectors differ for the G38 I _J_ (K_) command and the G41/G42 I_J_(K_) command.
G38 G41/G42
~ (G41)
~ G38 G91 X100. I50. J50. ;
~
~ (G41)
~ G41 G91 X100. I50. J50. ;
~
E xa
m pl
e
(I J)
(Compensation amount)
(I J) (Compensation amount)
Vector in IJ direction having a compensation amount size
Vector perpendicular in IJ direction and having a compensation amount size
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
199
(4) Refer to the following table for the offset methods based on the presence and/or absence of
the G41 and G42 commands and I, J, (K) command.
G41/G42 I, J (K) Offset method No No Intersection point calculation type vector No Yes Intersection point calculation type vector Yes No Intersection point calculation type vector
Yes Yes I, J, type vector No insertion block
N1 G91 G01 G41 X200. D1 F1000 ; N2 X-150. Y150. ; N3 G41 X300. I50. ; N4 X-150. Y-150. ; N5 G40 X-200. ; During the I, J type vector compensation, the A insertion block will not exist.
Y
X N5
(I,J)
N4
N3
N2
N1
A
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
200
12.4.4 Interrupts during Tool Radius Compensation
MDI interrupt
Tool radius compensation is valid in any automatic operation mode-whether tape, memory or MDI operation. An interrupt based on MDI will give the result as in the figure below after block stop during tape or memory operation. (1) Interrupt without movement (tool path does not change)
N2
S
N3
N1 G41D1;
N2 X20. Y50. ;
N3 G3 X40. Y-40. R70. ; S1000 M3;
MDI interrupt
(Stopping position for single block)
(2) Interrupt with movement
The offset vectors are automatically re-calculated at the movement block after interrupt.
N1 G41D1;
N2 X20. Y50. ;
N3 G3 X40.Y-40. R70. ; X50. Y-30. ;
X30. Y50. ;
With linear interrupt
S
S
N2 N3
MDI interrupt
S
S
N2 N3
N1 G41 D1 ;
N2 X20. Y50. ;
N3 G3 X40. Y-40. R70.; G2 X40. Y-40. R70. ;
G1 X40. ;
MDI interrupt
With circular interrupt
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
201
Manual interrupt
(1) Interrupt with manual absolute OFF.
The tool path is shifted by an amount equivalent to the interrupt amount.
Tool path after interrupt
Interrupt Tool path after compensation
Program path
(2) Interrupt with manual absolute ON.
In the incremental value mode, the same operation results as with manual absolute OFF. In the absolute value mode, however, the tool returns to its original path at the end point of the block following the interrupted block, as shown in the figure.
Interrupt
Interrupt
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
202
12.4.5 General Precautions for Tool Radius Compensation Precautions
(1) Designating the offset amounts
The offset amounts can be designated with the D code by designating an offset amount No. Once designated, the D code is valid until another D code is commanded. If an H code is designated, the program error (P170) No COMP No will occur. Besides being used to designate the compensation amounts for tool radius compensation, the D codes are also used to designate the compensation amounts for tool position compensation.
(2) Changing the offset amounts
Offset amounts are normally changed when a different tool has been selected in the compensation cancel mode. However, when an amount is changed in the compensation mode, the vectors at the end point of the block are calculated using the offset amount designated in that block.
(3) Offset amount symbols and tool center path
If the offset amount is negative (), the figure will be the same as if G41 and G42 are interchanged. Thus, the axis that was rotating around the outer side of the workpiece will rotate around the inner side, and vice versa. An example is shown below. Normally, the offset amount is programmed as positive (+). However, if the tool path center is programmed as shown in (a) and the offset amount is set to be negative (), the movement will be as shown in (b). On the other hand, if the program is created as shown in (b) and the offset amount is set to be negative (), the movement will be as shown in (a). Thus, only one program is required to execute machining of both male and female shapes. The tolerance for each shape can be randomly determined by adequately selecting the offset amount. (Note that a circle will be divided with type A when compensation is started or canceled.)
Workpiece
Workpiece
G41 offset amount (+) or G42 offset amount () (a)
Tool center path
G41 offset amount () or G42 offset amount (+) (b)
Tool center path
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
203
12.4.6 Changing of Compensation No. during Compensation Mode Function and purpose
As a principle, the compensation No. must not be changed during the compensation mode. If changed, the movement will be as shown below. When offset No. (compensation amount) is changed:
G41 G01 ……………………….. Dr1 ; ( = 0, 1, 2, 3) N101 G0 Xx1 Yy1 ; N102 G0 Xx2 Yy2 Dr2 ; …………………………….. Offset No. changed N103 Xx3 Yy3 ;
(1) During linear linear
Tool center path
Program path
The offset amount designated with N101 will be applied.
The offset amount designated with N102 will be applied.
Tool center path
Program path
N101 r2
r2r1
r1 N102
N103
r1
r1
r1 r1
r2
r2
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
204
(2) Linear circular
r1
r2
r1
N102
r1
r1
r1 r1
r2
Tool center path
Program path
Center of circular Tool center path
Program path
N101
N102 G02
N101
G03
Center of circular
(3) Circular circular
Tool center path
Program path
Center of circular
r1 N101
r1 r2
N102
r1 r1
r1 r1
r2
Center of circular
Center of circular
Center of circular
Tool center path Program path
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
205
12.4.7 Start of Tool Radius Compensation and Z Axis Cut in Operation Function and purpose
Often when starting cutting, a method of applying a radius compensation (normally the XY plane) beforehand at a position separated for the workpiece, and then cutting in with the Z axis is often used. When using this method, create the program so that the Z axis movement is divided into the two steps of rapid traverse and cutting feed after nearing the workpiece.
Example of program
When the following type of program is created:
Tool center path
N4: Z axis lowers (1 block)
N1 Y
X
N1 Y
Z
N4 N6 N6 N1 G91 G00 G41 X 500. Y 500. D1 ; N2 S1000 ; N3 M3 ; N4 G01 Z-300. F1 ; N6 Y 100. F2 ;
With this program, at the start of the N1 compensation the program will be read to the N6 block. The relation of N1 and N6 can be judged, and correct compensation can be executed as shown above. If the above program’s N4 block is divided into two
N1 G91 G00 G41 X 500. Y 500. D1; N2 S1000 ; N3 M3 ; N4 Z-250. ; N5 G01 Z-50. F1 ; N6 Y 100. F2 ; Cut in
N1
N1
N4
N5N6
X
Y Z
N6
X
In this case, the four blocks N2 to N5 do not have a command in the XY plane, so when the N1 compensation is started, the program cannot be read to the N6 block. As a result, the compensation is done based only on the information in the N1 block, and the compensation vector is not created at the start of compensation. Thus, an excessive cut in occurs as shown above.
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
206
In this case, consider the calculation of the inner side, and before the Z axis cutting, issue a command in the same direction as the direction that the Z axis advances in after lowering, to prevent excessive cutting.
N1 G91 G00 G41 X 500. Y 400. D1 ;
N2 Y100. S1000 ;
N3 M3 ;
N4 Z-250. ;
N5 G01 Z-50. F1 ;
N6 Y 100. F2 ;
N1 Y
Z
N5
N6
N2
N1
N2
Y
X
N6
N4
N6
The movement is correctly compensated as the same direction as the N6 advance direction is commanded in N2.
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
207
12.4.8 Interference Check Function and purpose
(1) Outline
A tool, whose radius has been compensated with the tool radius compensation function by the usual 2-block pre-read, may sometimes cut into the workpiece. This is known as interference, and interference check is the function which prevents this from occurring. There are three types of interference check, as indicated below, and each can be selected for use by parameter.
Function Parameter Operation Interference check alarm function
#8102 : OFF #8103 : OFF
A program error results before the execution of the block in which the cut arises, and operation stops.
Interference check avoidance function
#8102 : ON #8103 : OFF
The tool path is changed so that workpiece is not cut into.
Interference check invalid function
#8103 : ON Cutting proceeds unchanged even when it occurs. Use this for microscopic segment programs.
(Note) #8102 COLL. ALM OFF (interference check avoidance) #8103 COLL. CHK OFF (interference check invalid)
Detailed description
(Example)
Avoidance path
Outer diameter of tool
N1 N3
N2
(G41) N1 G90 G1 X50. Y-100.; N2 X70. Y-100.; N3 X120. Y0;
Cutting with N2 Cutting with N2
(1) With alarm function
The alarm occurs before N1 is executed and so, using the edit function, N1 can be changed as below and machining can be continued : N1 G90 G1 X20. Y40. ;
(2) With avoidance function
The intersection point of N1 and N3 is calculated and the interference avoidance vectors are created.
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
208
(3) With interference check invalid function
The tool passes while cutting the N1 and N3 line.
(4)'(3)'(2)
(2)'(1)
N1
N3
N2
(1)’
(3)
(4)
Example of interference check
Vectors (1) (4)’ check No interference Vectors (2) (3)’ check No interference Vectors (3) (2)’ check Interference Erase vectors (3) (2)’ Erase vectors (4) (1)’
With the above process, the vectors (1), (2), (3)’ and (4)’ will remain as the valid vectors, and the path that connects these vectors will be executed as the interference avoidance path.
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
209
Conditions viewed as interference
If there is a movement command in three of the five pre-read blocks, and if the compensation calculation vectors created at the contacts of each movement command intersect, it will be viewed as interference.
Tool center path Program path
Vectors intersect N1 N3
N2
r
When interference check cannot be executed
(1) When three of the movement command blocks cannot be pre-read (When there are three or more blocks in the five pre-read blocks that do not have movement) (2) When there is an interference following the fourth movement block
Tool center path
Program path
Interference check is not possible
N1
N3
N2
N4
N5
N6
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
210
Operation during interference avoidance
The movement will be as shown below when the interference avoidance check is used.
Tool center path Program path
N1 N3
N2
Solid line vector : Valid Dotted line vector : Invalid
Linear movement
Center of circular
Program path
Tool center path when interference is avoided
Tool center path without interference check
N1
N3N2
N1
N3N2
r
r
Tool center path when interference is avoided
Tool center path without interference check
Program path
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
211
If all of the line vectors for the interference avoidance are deleted, create a new avoidance vector as shown on the right to avoid the interference.
Avoidance vector 1 Avoidance vector 2
Tool center path 1
Tool center path 2
Avoidance vector
Tool center path
Program path
Program path
N1
N3
N2
N1
N3
N2
r1
N4
r2
r1 r2
Avoidance vector
In the case of the figure below, the groove will be left uncut.
Tool center path
Program path
Interference avoidance path
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
212
Interference check alarm
The interference check alarm occurs under the following conditions.
(1) When the interference check alarm function has been selected
(a) When all the vectors at the end block of its own block have been deleted. When, as shown in the figure, vectors 1 through 4 at the end point of the N1 block have all been deleted, program error (P153) results prior to N1 execution.
N1
2 3
N2 1
N3 4
(2) When the interference check avoidance function has been selected
(a) When there are valid vectors at the end point of the following block even when all the vectors at the end point of its own block have been deleted. (i) When, in the figure, the
N2 interference check is conducted, the N2 end point vectors are all deleted but the N3 end point vectors are regarded as valid. Program error (P153) now occurs at the N1 end point.
Alarm stop
N1
2 N21
N3 4 3
N4
(ii) In a case such as that
shown in the figure, the tool will move in the reverse direction at N2. Program error (P153) occurs after N1 execution.
N1
N2 N3
N4
1 2 3 4
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
213
(b) When avoidance vectors cannot be created
(i) Even when, as in the figure, the conditions for creating the avoidance vectors are met, it may still be impossible to create these vectors or the interference vectors may interfere with N3. Program error (P153) will occur at the N1 end point when the vector intersecting angle is more than 90.
Alarm stop
N1
N2
N3
N4
Alarm stop
Angle of intersection
N1
N2
N3
N4
(c) When the program advance direction and the advance direction after compensation are reversed In the following case, interference is still regarded as occurring even when there is actually no interference. When grooves which are narrower than the tool radius or which have parallel or widening walls are programmed
Tool center path
Program path
Stop
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
214
12.4.9 Diameter Designation of Compensation Amount Function and purpose
With this function, the tool radius compensation amount can be designated by tool diameter. When the control parameter #8117 OFS Diam DESIGN is ON, the compensation amount specified to the commanded tool No. will be recognized as the diameter compensation amount, and the amount will be converted to the radius compensation amount when executing the compensation.
Operations when designating the compensation amount with diameter
(1) When the tool radius compensation amount D=10.0 is commanded, tool radius compensation
amount «d» is 5.0 if the parameter «#8117» is ON (set to «1»). (Tool radius compensation amount «r» is 10.0 if the parameter «#8117» is OFF (set to «0»).)
Program path r
Program path
Tool center path (When #8117 is ON)
20 tool
d
Tool center path (When #8117 is OFF)
20 tool
(a) Linear to linear (acute angle)
Tool center path (When #8117 is OFF)
Tool center path (When #8117 is ON)d
s
r
d
r
Outside of the corner
d r
d
r
s
Inside of the corner
Program path
Program path
Tool center path (When #8117 is ON)
Tool center path (When #8117 is OFF)
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
215
(b) Linear to arc (obtuse angle)
Program path Program path
Tool center path (When #8117 is ON)
Tool center path (When #8117 is OFF)
s
Arc center
d
r
Inside of the corner
r
Arc center
s
d
Outside of the corner
(c) Arc to linear (obtuse angle)
d
s
r d s
r
d
Arc center
r
Program path
Program path
Tool center path (When #8117 is ON)
Tool center path (When #8117 is OFF)
Arc center
Inside of the corner Outside of the corner
Tool center path (When #8117 is ON)
Tool center path (When #8117 is OFF)
Restrictions
(1) If tool radius compensation amount has already been set, the compensation amount is not be
changed even if the parameter «8117» is changed.
(2) Make sure not to change the parameter #8117 during the compensation. When the parameter is changed using parameter input by program function, the program error (P241) will occur.
(3) If the parameter #8117 is set to ON with the parameter «#1037 cmdtyp» set to 2, the tool radius wear data is also regarded as the diameter compensation amount, thus, it will be converted to the radius value and compensation will be performed.
(4) Diameter designation of tool radius compensation amount can be used for the tool life management data.
(5) There is no effect by #8117 on the tool radius measurement function.
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
216
12.4.10 Workpiece Coordinate Changing during Radius Compensation Function and purpose
When the tool radius compensation is executed, the tool center path is calculated based on the position on the coordinate system. The based coordinate system can be changed by the parameter.
Detailed description
When the parameter is «0», the tool radius compensation is calculated based on the position on the workpiece coordinate system. When the parameter is «1», the tool radius compensation is calculated based on the position on the program coordinate system. The program coordinate systems are defined as shown in the figure below.
G52 Local coordinate system
Local coordinate system offset G54 to G59/G54.1Pn Workpiece coordinate system /Extended workpiece coordinate system
Workpiece coordinate system offset
G92 offset
Extended workpiece coordinate system offset /G54.2Pn Extended workpiece coordinate system offset
G53 Basic machine coordinate system Interrupt amount offset
1st reference position offset
1st reference position
Program coordinate system
12. Tool Compensation Functions 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42
217
The coordinate system changed by parameter is as follows. G90 G54 G00 X15. Y20. N1 G41 D3 X5. Y10.; N2 G01 Y-20. F1000; N3 G40 X30.; M30;
D3 = 5.000 G54 offset X15.000 Y15.000
Program coordinate system
G54
10.0
5.0
-20.0
20.0
(i) Parameter = 0
G53
N2
N3
N1
Compensation vector
Tool center path
Program path
Program path
G54
N2
N3
N1
25.0
-5.0
20.0 35.0
(ii) Parameter = 1
G53
Compensation vector
Tool center path
Program coordinate system
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42
218
12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42 Function and purpose
The three-dimensional tool radius compensation compensates the tool in a three-dimensional space following the commanded three-dimensional vectors.
Tool center coordinate position (x’, y’, z’)
Workpiece
Y (J) X (I)
Three-dimensional compensation vector
Z (K)
r: tool radius
Program coordinate position (x, y, z)
Plane normal line vector (I, J, K)
Tool
As shown above, the tool is moved to the tool center coordinate position (x’, y’, z’) which is offset by the tool radius «r» in respect to the program coordinate position (x, y, z) following the plane normal line vector (I, J, K). Though two-dimensional tool radius compensation creates the vectors at a right angle to the (I, J, K) direction, three-dimensional tool radius compensation creates the vector in the (I, J, K) direction. (The vector is created at the end point of the block.) The three-dimensional compensation vector (offset) axis elements are as the right.
I Hx = * r
(I2 + J2 + K2)
J HY = * r
(I2 + J2 + K2)
K HZ = * r
(I2 + J2 + K2)
Thus, the tool center coordinate position (x’, y’, z’) is each expressed as the right. Note that (x, y, z) are the program coordinate position.
x = x + Hx y = y + Hy z = z + Hz
(Note 1) Three-dimensional compensation vector (Hx, Hy, Hz) refers to the plane normal line
vector such as follows; The direction is same as the plane normal line vector (I, J, K ). The size equals to the tool radius «r».
(Note 2) When the machining parameter «#8071 3-D CMP» is set to a value other than «0», the value of «#8071 3-D CMP» will be used as the (I2 + J2 + K2) value. (Refer to the Setup Manual for details.)
(Note 3) This function is an additional specification. If commanded when the function is not provided, an error will occur.
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42
219
Command format
Command the compensation No. D and plane normal line vector (I, J, K) in the same block as the three-dimensional tool radius compensation command G41 (G42). If only one or two axes are commanded, the normal tool radius compensation mode will be applied. (When setting «0» to the axes, this command is valid.)
G41(G42) X__ Y__ Z__ I__ J__ K__ D__ ;
Three-dimensional tool radius compensation starts. — Refer to (Example 1) and (Example 2).
X__ Y__ Z__ I__ J__ K__; :
New plane normal line vector are commanded in the compensation mode. — Refer to (Example 3) to (Example 7).
G40; (or D00;) G40 X__ Y__ Z__; (or X__ Y__ Z__ D00;)
Three-dimensional tool radius compensation is canceled. — Refer to (Example and (Example 9).
G41 G42 G40 X, Y, Z I, J, K D
: Three-dimensional tool radius compensation command (+ direction) : Three-dimensional tool radius compensation command (- direction) : Three-dimensional tool radius compensation cancel command : Movement axis command compensation space : Plane normal line vector : Compensation No. (Note that when «D00» is issued, three dimensional tool radius compensation will be canceled even if G40 is not commanded.)
Compensation amount: Compensation
G code + D00
G40 Cancel Cancel Cancel G41 I, J, K direction Reverse direction of I, J, K Cancel G42 Reverse direction of I, J, K I, J, K direction Cancel
Detailed description
(Example)
G17 G41 Xx Yy Zz Ii Jj Kk ;
XYZ space
G17 ; G41 Yy Ii Jj Kk ;
XYZ space
G17 V ; G41 Xx Vv Zz Ii Jj Kk ;
XVZ space
G17 W ; G41 Ww Ii Jj Kk ;
XYW space
G17 ; G41 Xx Yy Zz Ww Ii Jj Kk ;
XYZ space
G17 W; G41 Xx Yy Zz Ww Ii Jj Kk ;
XYW space
G17 ; G41 Ii Jj Kk ;
XYZ space
The compensation space is determined by the axis address commands (X, Y, Z, U, V, W) of the block where the three-dimensional tool radius compensation starts. Here, U, V and W are each the additional axes for the X, Y and Z axis. If the X axis and U axis (Y and V, Z and W) are commanded simultaneously in the three-dimensional tool radius compensation start block, the currently commanded plane selection axis will have the priority. If the axis address is not commanded, it will be interpreted that the X, Y and Z axes are commanded for the coordinate axes.
G17 U ; G41 Ii Jj Kk ;
UYZ space
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42
220
Example of operation
(1) Compensation start: When there is a movement command
G41 xx Yy Zz Ii Jj Kk Dd ;
Program path
Three-dimensional compensation vector
Tool center path
Start point
(2) Compensation start: When there is no movement command
G41 Ii Jj Kk Dd ;
Three-dimensional compensation vector
Tool center path
Start point
(3) Movement during the compensation: When there is a movement command and a plane normal
line vector command
New vector
Old vector
Xx Yy Zz Ii Jj Kk ;
Program path
Tool center path
Start point
(4) Movement during the compensation: When there is no plane normal line vector command
Xx Yy Zz Ii Jj Kk ;
New vector Old vector
Program path
Tool center path
Start point
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42
221
(5) Movement during the compensation: For arc or helical cutting
The I, J, K commands for a circular or helical cutting are regarded as the circular center commands, thus, the new vector is equivalent to the old vector. Even for the R-designation method, commanded I, J, K addresses will be ignored, then the new vector will be equivalent to the old vector.
G02 Xx Yy (Zz) Ii Jj ; I, J(K) means the circular center or
G02 Xx Yy (Zz) Rr ; R-designated circular
New vector Old vector
Program path
Tool center path
Start point
(Note) The center coordinate will not shift during the circular or helical cutting.
Thus, when I, J, K are commanded with the vector as below, the program error (P70) will occur.
Circular radius
Circular center
G02 Xx Yy (Zz) Ii Jj ; I, J(K) means the circular center or
G02 Xx Yy (Zz) Rr ; R-designated circular
New vector Old vector
Program path
Tool center path
Start point
Circular radius
(6) Movement during the compensation: When compensation amount is to be changed
G41 Xx Yy Zz Ii Jj Kk Dd1 ; : G41 Xx Yy Zz Ii Jj Kk Dd2 ;
New vector
Program path
Old vector
Start point
Tool center path
(Note 1) If I, J, K are not commanded in a block where the compensation amount is to be changed,
the vector will be equivalent to the old vector. In this case, the modal will change, however, the compensation amount will change when I, J, K are commanded.
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42
222
(7) Movement during the compensation: When compensation direction is to be changed
G41 Xx Yy Zz Ii Jj Kk Dd1 ; : G42 Xx Yy Zz Ii Jj Kk ; New vector
Program path Old vector
Start point
Tool center path
(Note 1) If I, J and K are not commanded in a block where the compensation direction is to be
changed, the vector will be equivalent to the old vector and the compensation direction will not be changed. In this case, the modal will change, however, the compensation direction will change when I, J and K are commanded.
(Note 2) If the compensation direction is changed in an arc (G02/G03) block, I, J will be the center of arc, thus, the compensation direction will not change. Even for the R-designation method, commanded I, J and K will be ignored, and the compensation direction cannot be changed.
(8) Compensation cancel: When there is a movement command
G40 Xx Yy Zz ; (or Xx Yy Zz D00
Program path
Old vector
Start point
Tool center path
End point
(9) Compensation cancel: When there is no movement command
G40; ( or D00
Program path
Old vector Tool center path
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42
223
Relation with other functions
(1) Normal tool radius compensation
If the plane normal line vector (I, J, K) is not commanded for all three axes in the three-dimensional tool radius compensation start block, the normal tool radius compensation mode will take place. If G41 (G42) is commanded without commanding the plane normal line vector during three-dimensional tool radius compensation, the modal will change, however, the old vector will be used. If G41 (G42) with the plane normal line vector is commanded during tool radius compensation, this command will be ignored and the normal tool radius compensation will take place.
(2) Tool length offset
Tool length offset is applied on the coordinate after three-dimensional tool radius compensation.
(3) Tool position offset
Tool position offset is applied on the coordinate after three-dimensional tool radius compensation.
(4) Fixed cycle
The program error (P155) will occur.
(5) Scaling Scaling is applied on the coordinate before three-dimensional tool radius compensation. Scaling is not applied on the plane normal line vector (I, J, K).
D1=10.
G90 ; G51 X0 Y0 P0.5 ; N1 G41 D1 X-10. Y-20. Z-10. I-5. J-5. K-5. ; N2 X-30. Y-30. Z-20. ; N3 X-50. Y-20. Z-10. ; N4 Y0. ;
N1( -5.000, -10.000, -10.000 ) N1( -10.773, -15.773, -15.773 )
N2( -15.000, -15.000, -20.000 ) N2( -20.773, -20.773, -25.773 )
N3( -25.000, -10.000, -10.000 ) N3( -30.773, -15.773, -15.773 )
N4( -25.000, 0.000, -10.000 ) N4( -30.773, -5.773, -15.773 )
*Upper: Program position after scaling Lower: Position after scaling and compensation
Program path
Path after compensation
Plane normal line vector
Program path
Path after compensation
Plane normal line vector
Program path after scaling
Path after scaling and compensation
Program path after scaling
Path after scaling and compensation
X
X
Y
Z
-50. -30. -20. -10.
-30.
-20.
-10.
-20.
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42
224
(6) Program coordinate rotation
Program coordinate rotation is executed in respect to the coordinates before three-dimensional tool radius compensation. The plane normal line vector (I, J, K) dose not rotate.
D1=10.
G90 ; G68 X0 Y0 R45. ; N1 G41 D1 X-10. Y-20. Z-10. I-5. J-5. K-5. ; N2 X-30. Y-30. Z-20. ; N3 X-50. Y-20. Z-10. ; N4 Y0. ;
N1( 7.071, -21.213, -10.000 ) N1( 1.298, -26.986, -15.773 )
N2( 0.000, -42.426, -20.000 ) N2( -5.773, -48.199, -25.773 )
N3( -21.213, -49.497, -10.000 ) N3( -26.986, -55.270, -15.773 )
N4( -35.355, -35.355, -10.000 ) N4( -41.128, -41.128, -15.773 )
*Upper: Program position after coordinate rotation Lower: Position after coordinate rotation and compensation
Program path after coordinate rotation
Path after coordinate rotation and compensation
X
Z
-20.
-10.
X
Y
-50. -30. -20. -10.
-30.
-20.
Program path
Path after compensation Plane normal line vector
Program path
Path after compensation
Plane normal line vector
Program path after coordinate rotation
Path after coordinate rotation and compensation
(7) Parameter coordinate rotation
Parameter coordinate rotation is applied on the coordinates after three-dimensional tool radius compensation. The plane normal line vector (I, J, K) rotates.
(8) Mirror image
Mirror image is applied on the coordinates after three-dimensional tool radius compensation. Mirror image is applied on the plane normal line vector (I, J, K).
(9) Skip
The program error (P608) will occur.
(10) Reference position check The compensation amount will not be canceled. Thus, if this is commanded during three-dimensional tool radius compensation, the path will be deviated by the compensation amount, so the program error (P434) will occur.
(11) Automatic corner override
Automatic corner override is invalid during three-dimensional tool radius compensation.
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42
225
(12) Machine coordinate system selection
(a) For the absolute command, all axes will be temporarily canceled at the commanded
coordinate position. D1=10.
G90 ; N1 G41 D1 X-10. Y-20. Z-10. I-5. J-5. K-5. ; N2 X-30. Y-30. Z-20. ; N3 X-50. Y-20. Z-10. ; N4 G53 Y0 ;
N1( -10.000, -20.000, -10.000 ) N1( -15.773, -25.773, -15.773 )
N2( -30.000, -30.000, -20.000 ) N2( -35.773, -35.773, -25.773 )
N3( -50.000, -20.000, -10.000 ) N3( -55.773, -25.773, -15.773 )
N4( -50.000, 0.000, -10.000 ) N4( -50.000, 0.000, -10.000 )
*Upper: Program position Lower: Position after compensation
Program path
Path after compensation
Program path
Path after compensation
X
X
Y
Z
-50. -30. -20. -10.
-30.
-20.
-10.
-20.
(b) For the incremental command, the axis will move by the amount obtained by subtracting
each axis vector from the incremental movement amount. (The compensation amount is temporarily canceled.) D1=10.
G91 ; N1 G41 D1 X-10. Y-20. Z-10. I-5. J-5. K-5. ; N2 X-20. Y-10. Z-10. ; N3 X-20. Y10. Z10. ; N4 G53 Y20. ;
N1( -10.000, -20.000, -10.000 ) N1( -15.773, -25.773, -15.773 )
N2( -30.000, -30.000, -20.000 ) N2( -35.773, -35.773, -25.773 )
N3( -50.000, -20.000, -10.000 ) N3( -55.773, -25.773, -15.773 )
N4( -50.000, 0.000, -10.000 ) N4( -50.000, 0.000, -10.000 ) *Upper: Program position Lower: Position after compensation
X
X
Y
Z
-50. -30. -20. -10.
-30.
-20.
-10.
-20.
Program path
Path after compensation
Program path
Path after compensation
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42
226
(13) Coordinate system setting
When commanded in the same block as the coordinate system setting, the coordinate system will be set, and operation will start up independently with the plane normal line vector (I, J, K). D1=10. G91 ; N1 G92 G41 D1 X-10. Y-20. Z-10. I-5. J-5. K-5. ; N2 X-20. Y-10. Z-10. ; N3 X-30. Y-10. Z10. ; N4 Y20. ; N1( -10.000, -20.000, -10.000 ) N1( -15.773, -25.773, -15.773 ) N2( -30.000, -30.000, -20.000 ) N2( -35.773, -35.773, -25.773 ) N3( -50.000, -20.000, -10.000 ) N3( -55.773, -25.773, -15.773 ) N4( -50.000, 0.000, -10.000 ) N4( -55.773, -5.773, -15.773 ) *Upper:
Program position Lower:
Position after compensation
Program path
Path after compensation
Program path
Path after compensation
X
X
Y
Z
-50. -30. -20. -10.
-30.
-20.
-10.
-20.
W(0,0)
W(0,0)
G92
G92
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42
227
(14) Reference position return
All the axes will be temporarily canceled at the intermediate point. D1=10.
G91 ; N1 G41 D1 X-10. Y-20. Z-10. I-5. J-5. K-5. ; N2 X-20. Y-10. Z-10. ; N3 X-20. Y10. Z10. ; N4 G28 X0 Y0 Z0 ;
N1( -10.000, -20.000, -10.000 ) N1( -15.773, -25.773, -15.773 )
N2( -30.000, -30.000, -20.000 ) N2( -35.773, -35.773, -25.773 )
N3( -50.000, -20.000, -10.000 ) N3( -55.773, -25.773, -15.773 )
N4( 0.000, 0.000, 0.000 ) N4( 0.000, 0.000, 0.000 )
N4( 20.000, 10.000, 10.000 ) N4( 20.000, 10.000, 10.000 ) *Upper: Program position (workpiece coordinate) Lower: Position after compensation
X
X
Z
-30. -20. -10.
-40.
-20.
-10.
-30.
W(0,0)
M(0,0)
-10.
Y
-30.
-20.
M(0,0)
W(0,0)
-20.
-10.
-50.
-30. -20. -70. -50.
Program path
Path after compensation
Program path
Path after compensation
(15) NC reset
Three-dimensional tool radius compensation will be canceled if NC reset is executed during three-dimensional tool radius compensation.
(16) Emergency stop
Three-dimensional tool radius compensation will be canceled by the emergency stop or emergency stop cancel during three-dimensional tool radius compensation.
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42
228
Restrictions
(1) The compensation No. is selected with the D address, however, the D address is valid only
when G41 or G42 is commanded. If D is not commanded, the number of the previous D address will be valid.
(2) Switch the mode to the compensation mode in the G00 or G01 mode. When changed during
the arc mode, the program error (P150) will occur. The compensation direction and compensation amount after the mode change will become valid from the block where I, J and K are commanded in the G00 or G01 mode. If three-dimensional tool radius compensation is commanded in a block not containing the plane normal line vector (I, J, K) during the arc mode, only the modal information will be changed. The plane normal line vector will be validated from the block where I, J and K are commanded next.
(3) During the three-dimensional tool radius compensation mode in a certain space, it is not
possible to switch the space to another one and to execute three-dimensional tool radius compensation. To switch the compensation space, always cancel the compensation mode with G40 or D00 first.
(Example) G41 Xx Yy Zz Ii Jj Kk; : :
Compensation starts in X, Y, Z space.
G41 Uu Yy Zz Ii Jj Kk; Compensation is carried out in X, Y, Z space, and U axis moves by commanded value.
(4) If the compensation No. D is other than the range of 1 to 40 with the standard specifications or
1 to 800 (max.) with the additional specifications, the program error (P170) will occur.
(5) Only the G40 and D00 commands can be used to cancel three-dimensional tool radius compensation.
(6) If the size (I2+J2+K2) of the vector commanded with I, J and K overflows, the program error
(P35) will occur.
12. Tool Compensation Functions 12.6 Tool Position Offset; G45 to G48
229
12.6 Tool Position Offset; G45 to G48 Function and purpose
Using the G45 to G46 commands, the movement distance of the axes specified in the same block can be extended or reduced by a preset compensation length. Furthermore, the compensation amount can be similarly doubled (x 2 expansion) or halved (x 2 reduction) with commands G47 and G48. The number of sets for the compensation differ according to machine specification. Refer to Specifications Manual.
D01 to Dn (The numbers given are the total number of sets for tool length compensation, tool position offset and Tool radius compensation.)
G45 command G46 command G47 command G48 command Expansion by
compensation amount only
Reduction by compensation amount
only
2 expansion by compensation amount
2 reduction by compensation amount
Internal arithmetic processing
Movement amount
Start point End point
Internal arithmetic processing
Movement amount
Start point End point
Internal arithmetic processing
Movement amount
Start point End point
Internal arithmetic processing
Movement amount
Start point End point
(Program command value)
=
(compensation amount) (Movement amount after compensation)
Command format
G45 X__ Y__ Z__ D__ ;
Expansion of movement amount by compensation amount set in compensation memory
G46 X__ Y__ Z__ D__ ; Reduction of movement amount by compensation amount set in compensation memory
G47 X__ Y__ Z__ D__ ; Expansion of movement amount by double the compensation amount set in compensation memory
G48 X__ Y__ Z__ D__ ; Reduction of movement amount by double the compensation amount set in compensation memory
X, Y, Z : Movement amount of each axis
D : Tool compensation No.
12. Tool Compensation Functions 12.6 Tool Position Offset; G45 to G48
230
Detailed description
Details for incremental values are given below.
Command
Movement amount of equivalent command
(assigned compensation amount = l)
Example (when X = 1000)
G45Xx Dd X ( x + l ) l = 10 X = 1010 l = 10 X = 990
G45Xx Dd X ( x + l ) l = 10 X = 1010 l = 10 X = 990
G46Xx Dd X ( x l ) l = 10 X = 990 l = 10 X = 1010
G46Xx Dd X ( x l ) l = 10 X = 990 l = 10 X = 1010
G47Xx Dd X ( x + 2 l ) l = 10 X = 1020 l = 10 X = 980
G47Xx Dd X ( x + 2 l ) l = 10 X = 1020 l = 10 X = 980
G48Xx Dd X ( x 2 l ) l = 10 X = 980 l = 10 X = 1020
G48Xx Dd X ( x 2 l ) l = 10 X = 980 l = 10 X = 1020
Precautions
(1) These commands should be used when operation is not in a canned cycle mode. (They are ignored even if they are assigned during a canned cycle.) (2) As a result of the internal arithmetic processing based on the expansion or reduction, the tool
will proceed to move in the opposite direction when the command direction is reversed.
Start point
End point Programmed command Compensation Tool movement
G48X20.000D01; Compensation amount = +15.000 Actual movement = X 10.000
(3) When a zero movement amount has been specified in the incremental value command (G91) mode, the result is as follows.
Compensation number : D01 Compensation amount corresponding to D01: 1234
NC command G45X0 D01; G45X 0 D01; G46X0 D01; G46X 0 D01; Equivalent command X1234; X 1234; X 1234; X1234;
When a zero movement amount has been specified with an absolute value command, the operation is completed immediately and the tool does not move for the compensation amount.
12. Tool Compensation Functions 12.6 Tool Position Offset; G45 to G48
231
(4) In the case of circular interpolation, cutter compensation is possible using the G45 to G48 commands only for one quadrant, two quadrants (semi-sphere) or three quadrants when the start and end points are on the axis.
The commands are assigned as follows depending on whether the compensation is applied for outside or inside the arc programmed path. However, in this case, compensation must already be provided in the desired direction at the arc start point. (If a compensation command is assigned for the arc independently, the arc start point and end point radii will shift by an amount equivalent to the compensation amount.)
Programed path 1/4 circle
G45
G46
G45 for compensation outside the circle G46 for compensation inside the circle
1/2 circle
Programmed path
G47
G48
G47 for compensation outside the circle G48 for compensation inside the circle
Programmed path
3/4 circle G45
G46 G45 for compensation outside the circle G46 for compensation inside the circle
12. Tool Compensation Functions 12.6 Tool Position Offset; G45 to G48
232
Example of program
(Example 1)
Tool position offset with 1/4 arc command
Programmed path 1000
Tool nose center path
200
X Start point 1000Programmed arc
center
End point
Y
Tool
It is assumed that compensation has already been provided in the + X direction by
D01 = 200.
G91 G45 G03 X-1000 Y1000 I-1000 F1000 D01;
Even if the compensation numbers are not assigned in the same block as the G45 to G48 commands, compensation is provided with the tool position compensation number previously stored in the memory. Program error «P170» results when the specified compensation number has exceeded the specification range. These G codes are unmodal and are effective only in the command block. Even with an absolute value command, the amount of the movement is extended or reduced for each axis with respect to the direction of movement from the end point of the preceding block to the position assigned by the G45 to G48 block. In other words, even for an absolute value command, compensation can be applied to movement amounts (incremental values) in the same block.
12. Tool Compensation Functions 12.6 Tool Position Offset; G45 to G48
233
When a command for «n» number of simultaneous axes is given, the same compensation will be applied to all axes. It is valid even for the additional axes (but it must be within the range of the number of axes which can be controlled simultaneously.)
Programmed end point
110. 50.
220.
50.
270. X
End point after compensation
G01 G45X220. Y60. D20 ; (D20) = +50. 000
60.
Y
Start point
(Note 1) If compensation is applied to two axes, over-cutting or under-cutting will result, as shown in the figures below. In cases like this, use the cutter compensation commands (G40 to G42).
Tool nose center path
Tool
Desired shape
Under-cutting
Programmed path
X
l: compensation amount setting
G01 G45 Xx1 Dd1 ; Xx2 Yy2 ;
G45 Yy3 ;
Y
Workpiece
Machined shape
l
l: compensation amount setting
G01 Xx1 ; G45 Xx2 Yy2 Dd2 ;
Yy3 ;
Tool nose center path
Tool
Desired shape
Over-cutting
Programmed path
X
Y
Workpiece
Machined shape
l
12. Tool Compensation Functions 12.6 Tool Position Offset; G45 to G48
234
(Example 2)
N1 G46 G00 Xx1 Yy1 Dd1 ;
N2 G45 G01 Yy2 Ff2 ;
N3 G45 G03 Xx3 Yy3 Ii3 ;
N4 G01 Xx4 ;
Tool nose center path
N3
Programmed path
X
Y
N4
N1
N2
(Example 3)
When the G45 to G48 command is assigned, the compensation amount for each pass is the amount assigned by the compensation number, and the tool does not move for the difference from the previous compensation as it would do with the tool length compensation command (G43).
Tool nose center path
40
Programmed path
30
N101
10
N102
30
30
30
40
40
10
N100
N105 N108N110
N103
N115
N114
N116
N113 N109
N112
N104
N106
N107
20R
10R
Start point
10R
N111
12. Tool Compensation Functions 12.6 Tool Position Offset; G45 to G48
235
Compensation amount D01 = 10.000mm (Offset amount of tool radius)
N100 G91 G46 G00 X40.0 Y40.0 D01 ; N101 G45 G01 X100.0 F200 ; N102 G45 G03 X10.0 Y10.0 J10.0 ; N103 G45 G01 Y40.0 ; N104 G46 X0 ; N105 G46 G02 X20.0 Y20.0 J20.0 ; N106 G45 G01 Y0 ; N107 G47 X30.0 ; N108 Y30.0 ; N109 G48 X30.0 ; N110 Y 30.0 ; N111 G45 X30.0 ; N112 G45 G03 X10.0 Y10.0 J10.0 ; N113 G45 G01 Y20.0 ; N114 X10.0 ; N115 Y40.0 ; N116 G46 X40.0 Y40.0 ; N117 M02 ; %
12. Tool Compensation Functions 12.7 Programmed Compensation Input ; G10, G11
236
12.7 Programmed Compensation Input ; G10, G11
Function and purpose
The tool compensation and workpiece offset can be set or changed on the tape using the G10 command. During the absolute value (G90) mode, the commanded compensation amount will become the new compensation amount, and during the incremental value (G91) mode, the commanded compensation amount will be added to the currently set compensation amount to create the new compensation amount.
Command format
(1) Workpiece offset input
G90 G10 L2 P__X__Y__Z__; G91 P : 0 External workpiece 1 G54 2 G55 3 G56 4 G57 5 G58 6 G59
(Note) The offset amount in the G91 will be an incremental amount and will be cumulated each time the program is executed. Command G90 or G91 before the G10 as a cautionary means to prevent this type of error.
(2) Tool compensation input
(a) For tool compensation memory I
G10 L10 P__R__ ; P : Compensation No. R : Compensation amount
(b) For tool compensation memory II
G10 L10 P__R__ ; Tool length compensation shape compensation G10 L11 P__R__ ; Tool length compensation wear compensation G10 L12 P__R__ ; Tool radius shape compensation G10 L13 P__R__ ; Tool radius wear compensation
(3) Offset input cancel
G11 ;
12. Tool Compensation Functions 12.7 Programmed Compensation Input ; G10, G11
237
Detailed description
(1) Program error (P171) will occur if this command is input when the specifications are not
available. (2) G10 is an unmodal command and is valid only in the commanded block. (3) The G10 command does not contain movement, but must not be used with G commands other
than G54 to G59, G90 or G91. (4) Do not command G10 in the same block as the fixed cycle and sub-program call command.
This will cause malfunctioning and program errors. (5) The workpiece offset input command (L2 or L20) should not issued in the same block as the
tool compensation input command (L10). (6) If an illegal L No. or compensation No. is commanded, the program errors (P172 and P170)
will occur respectively. If the offset amount exceeds the maximum command value, the program error (P35) will occur. (7) Decimal point inputs can be used for the offset amount. (8) The offset amounts for the external workpiece coordinate system and the workpiece
coordinate system are commanded as distances from the basic machine coordinate system zero point.
(9) The workpiece coordinate system updated by inputting the workpiece coordinate system will follow the previous modal (G54 to G59) or the modal (G54 to G59) in the same block.
(10) L2 (or L20) can be omitted when the workpiece offset is input. (11) If the P command is omitted at the workpiece offset input, the currently selected workpiece
offset will be handled as the input.
Example of program
(1) Input the compensation amount
; G10L10P10R12345 ; G10L10P05R98765 ; G10L10P30R2468 ;
H10=-12345 H05=98765 H30=2468
(2) Updating of compensation amount
(Example 1) Assume that H10 = -1000 is already set. N1 G01 G90 G43 Z — 100000 H10; (Z = -101000) N2 G28 Z0;
N3 G91 G10 L10 P10R — 500 ; (The mode is the G91 mode, so -500 is added.)
N4 G01 G90 G43 Z — 100000 H10 ; (Z = -101500)
12. Tool Compensation Functions 12.7 Programmed Compensation Input ; G10, G11
238
(Example 2) Assume that H10 = -1000 is already set.
Main program N1 G00 X100000 ;a N2 #1 = -1000 ; N3 M98 P1111 L4 ;b1, b2, b3, b4
Subprogram O1111 N1 G01 G91 G43 Z0 H10 F100 ; c1, c2, c3, c4 G01 X1000 ; d1, d2, d3, d4 #1 = #1 1000 ; G90 G10 L10 P10 R#1 ; M99;
(Note) Final offset amount will be H10= -5000.
(a) (b1) (b2) (b3) (b4)
1000 1000 1000 1000
10 00
1 00
0 10
00 1
00 0 c1
d1
c3 d3
c2 d2
c4 d4
(Example 3) The program for Example 2 can also be written as follows. Main program N1 G00 X100000 ; N2 M98 P1111 L4 ;
Subprogram O1111 N1 G01 G91 G43 Z0 H10 F100 ; N2 G01 X1000 ; N3 G10 L10 P10 R1000 ; N4 M99 ;
12. Tool Compensation Functions 12.7 Programmed Compensation Input ; G10, G11
239
(3) When updating the workpiece coordinate system offset amount
Assume that the previous workpiece coordinate system offset amount is as follows. X = 10.000 Y = 10.000
N100 G00 G90 G54 X0 Y0 ; N101 G90 G10 L2 P1 X15.000 Y15.000 ; N102 X0 Y0 ; M02 ;
Basic machine coordinate system zero point
G54 coordinate before change
G54 coordinate after change
-X -20. -10.
-10.
M
-20.
-Y
-Y
-Y
-X
-X
N100
N101
N102
(W1)
W1
(Note 1) Changes of workpiece position display at N101
At N101, the G54 workpiece position display data will change before and after the workpiece coordinate system is changed with G10.
X = 0 X = +5.000 Y = 0 Y = +5.000
When workpiece coordinate system offset amount is set in G54 to G59
G90 G10 L2 P1 X10.000 Y10.000 ; G90 G10 L2 P2 X20.000 Y20.000 ; G90 G10 L2 P3 X30.000 Y30.000 ; G90 G10 L2 P4 X40.000 Y40.000 ; G90 G10 L2 P5 X50.000 Y50.000 ; G90 G10 L2 P6 X60.000 Y60.000 ;
12. Tool Compensation Functions 12.7 Programmed Compensation Input ; G10, G11
240
(4) When using one workpiece coordinate system as multiple workpiece coordinate
systems
#1 = 50. #2 = 10. ; M98 P200 L5 ; M02 ; % N1 G90 G54 G10 L2 P1 X#1 Y#1 ; N2 G00 X0 Y0 ; N3 X5. F100 ; N4 X0 Y5. ; N5 Y0 ; N6 #1 = #1 + #2 ; N7 M99 ; %
Main program
Subprogram O200
Basic machine coordinate system zero point
4th time
3rd time
2nd time
1st time
-X -10.
-10.
M
-20.
-Y -50.
-30.
-60.
-40.
G54″»
W
W
W
W
W
G54″‘
G54″
G54′
G54
-50. -40. -30. -20.
5th time
Precautions
(1) Even if this command is displayed on the screen, the offset No. and variable details will not be
updated until actually executed. N1 G90 G10 L10 P10R100 ; N2 G43 Z10000 H10 ; N3 G0 X-10000 Y10000 ; N4 G90 G10 L10 P10 R200 ;…The H10 offset amount is updated when the N4 block is
executed.
12. Tool Compensation Functions 12.8 Inputting the Tool Life Management Data; G10, G11
241
12.8 Inputting the Tool Life Management Data; G10, G11 12.8.1 Inputting the Tool Life Management Data by G10 L3 Command
Function and purpose
Using the G10 command (unmodal command), the tool life management data can be registered, changed and added to, and preregistered groups can be deleted.
Command format
(1) Registering data
G10 L3 ; Start of life management data registration P_L_Q_; Registration of the group No., the life, the control
method T_H_D_; Registration of the tool No., the length compensation
No., the radius compensation No. T_H_D_; P_L_Q_; Registration of next group No., the life, the control
method T_H_D_; Registration of the tool No., the length compensation
No., the radius compensation No. G11 ; End of life management data registration P :Group No. L :Life Q :Control method T :Tool No., The spare tools are selected in the order of the tool numbers
registered here. H :Length compensation No. D :Radius compensation No.
Next group
First group
(2) Changing and adding groups
G10 L3 P1; Start of life management data change or addition P_L_Q_; Change or addition of the group No., the life,
the control method T_H_D_; Change or addition of the tool No., the length
compensation No., the radius compensation No. T_H_D_; P_L_Q_; Change or addition of next group No., the life,
the control method T_H_D_; Change or addition of the tool No., the length
compensation No., the radius compensation No. G11 ; End of life management data change or addition P : Group No. L : Life Q : Control method T : Tool No. H : Length compensation No. D : Radius compensation No.
Next group
First group
(3) Deleting a group
G10 L3 P2; Start of life management data deletion P_; Delete the group No. P_; Delete next group No. G11 ; End life management data deletion P : Group No.
12. Tool Compensation Functions 12.8 Inputting the Tool Life Management Data; G10, G11
242
Example of operation
Program example Operation Data registration
G10 L3; P10 L10 Q1; T10 H10 D10; G11; M02 ;
1. After deleting all group data, the registration starts. 2. Group No. 10 is registered. 3. Tool No. 10 is registered in group No. 10. 4. The registration ends. 5. The program ends.
Group change, addition
G10 L3 P1; P10 L10 Q1; T10 H10 D10; G11; M02 ;
1. Changing and addition of the group and tool starts. 2. The change and addition operation takes place in the following manner.
(1) When group No. 10 has not been registered. Group No. 10 is additionally registered. Tool No. 10 is registered in group No. 10.
(2) When group No. 10 has been registered, but tool No. 10 has not been registered. Tool No. 10 is additionally registered in group
No. 10. (3) When group No. 10 and tool No. 10 have been
both registered. The tool No. 10 data is changed.
3. The group and tool change and addition ends. 4. The program ends.
Group deletion
G1 L3 P2; P10; G11; M02 ;
1. The group deletion starts. 2. The group No. 10 data is deleted. 3. The group deletion ends. 4. The program ends.
Command range
Item Command range Group No. (Pn) 1 to 99999999 Life (Ln) 0 to 9999 times (No. of times control method)
0 to 4000 minutes (time control method) Control method (Qn) 1 to 3
1: Number of mounts control 2: Time control 3: Number of cutting times control
Tool No. (Tn) 1 to 99999999 Length compensation No. (Hn) 0 to 999 Radius compensation No. (Dn) 0 to 999
12. Tool Compensation Functions 12.8 Inputting the Tool Life Management Data; G10, G11
243
12.8.2 Inputting the Tool Life Management Data by G10 L30 Command
Function and purpose
Using the G10 command (unmodal command), the tool life management data can be registered, changed and added to, and preregistered groups can be deleted. Registering data To specify absolute value compensation amount or increment value compensation amount by control method, the length compensation and diameter compensation can be registered/changed with the tool compensation amount format.
Command format
(1) Registering data
G10 L30 ; Start of life management data registration P_L_Q_; Registration of the group No., the life, the control
method T_H_R_; Registration of the tool No., the length compensation
(No./amount), the radius compensation (No./amount) T_H_R_; P_L_Q_; Registration of next the group No., the life, the control
method T_H_R_; Registration of the tool No., the length compensation
(No./amount), the radius compensation (No./amount) G11 ; End of data registration for life management P :Group No. L :Life Q :Control method T :Tool No., he spare tools are selected in the order of the tool Nos. registered
here. H :Length compensation No. or length compensation amount R :Length diameter compensation No. or diameter compensation amount
Next group
First group
(2) Changing and adding groups
G10 L30 P1; Start of life management data change or addition P_L_Q_; Change or addition of the group No., the life,
the control method T_H_R_; Change or addition of the tool No., the length
compensation (No./amount), the radius compensation (No./amount)
T_H_R_; P_L_Q_; Change or addition of the group No., the life,
the control method T_H_R_; Change or addition of the tool No., the length
compensation (No./amount), the radius compensation (No./amount)
G11 ; End of life management data change or addition P L Q T H R
: Group No. : Life : Length compensation data format, radius compensation data format, control method : Tool No. : Length compensation No. or length compensation amount : Length diameter compensation No. or diameter compensation amount
Next group
First group
12. Tool Compensation Functions 12.8 Inputting the Tool Life Management Data; G10, G11
244
(3) Deleting a group
G10 L30 P2; Start of life management data deletion P_; Delete the group No. P_; Delete next group No. G11 ; End life management data deletion P : Group No.
Example of operation
Program example Operation
Data registration
G10 L30 ; P10 L10 Q001 ; T10 H10 R10 ; G11 ; M02 ;
1. After deleting all group data, the registration starts. 2. Group No. 10 is registered.
Tool management method is number of mounts Compensation No. method is applied to tool length compensation and tool radius compensation.
3. Tool No. 10 is registered in group No. 10. 4. The registration ends. 5. The program ends.
Group change, addition
G10 L30 P1 ; P10 L10 Q122 ; T10 H10 R0.25 ; G11; M02 ;
1. Changing and addition of the group and tool starts. 2. The change and addition operation takes place in the
following manner. (1) When group No. 10 has not been registered.
(a) Group No. 10 is additionally registered. The change and addition tool Tool management method is number of usages Tool length compensation is incremental value
compensation amount method Tool radius compensation is absolute value
compensation amount method (b) Tool No. 10 is registered in group No. 10. The absolute value compensation amount «0.25» is set to tool radius compensation.
(2) When group No. 10 has been registered, but tool No. 10 has not been registered.
Tool No. 10 is additionally registered in group No. 10. (3) When group No. 10 and tool No. 10 have been both
registered. The tool No. 10 data is changed.
3. The group and tool change and addition ends. 4. The program ends.
Group deletion
G10 L30 P2 ; P10 ; G11 ; M02 ;
1. The group deletion starts. 2. The group No. 10 data is deleted. 3. The group deletion ends. 4. The program ends.
12. Tool Compensation Functions 12.8 Inputting the Tool Life Management Data; G10, G11
245
Command range
Item Command range Group No. (Pn) 1 to 99999999 Tool No. (Tn) 1 to 99999999 Control method (Qabc) abc : Three integer digits
a. Tool length compensation data format 0: Compensation No. 1: Incremental value compensation amount 2: Absolute value compensation amount
b. Tool radius compensation data format 0: Compensation No. 1: Incremental value compensation amount 2: Absolute value compensation amount
c. Tool management method 0: Usage time 1: Number of mounts 2: Number of usages
Life (Ln) 0 to 4000 minutes (usage time) 0 to 9999 times (number of mounts) 0 to 9999 times (number of usages)
Length compensation (No./amount)
(Hn) 0 to 999 (compensation No.) 9999.999 (incremental value compensation amount) 9999.999 (absolute value compensation amount)
Radius compensation (No./amount)
(Dn) 0 to 999 (compensation No.) 9999.999 (incremental value compensation amount) 9999.999 (absolute value compensation amount)
12. Tool Compensation Functions 12.8 Inputting the Tool Life Management Data; G10, G11
246
12.8.3 Precautions for Inputting the Tool Life Management Data
Precautions
(1) The tool life data is registered, changed, added to or deleted by executing the program in the
memory or MDI mode. (2) The group No. and tool No. cannot be commanded in duplicate. (3) When two or more addresses are commanded in one block, the latter address will be valid. (4) If the life data (L_) is omitted, the life data for that group will be «0». (5) If the control method (Q_) is omitted, the control method for that group will follow the base
specification parameter «#1106 Tcount». Note that when carrying out the No. of cutting times control method, command the method from the program.
(6) If the control method (Q_) is not designated with 3-digit by G10 L30 command, the omitted high-order are equivalent to «0». Therefore, «Q1» is equivalent to «Q001», and «Q12» is equivalent to «Q012».
(7) If the length compensation No. (H_) is omitted, the length compensation No. for that group will be «0».
(8) If the radius compensation No. (D_) is omitted, the radius compensation No. for that group will be «0».
(9) Programming with a sequence No. is not possible between G10 L3 or G10 L30 and G11. Program error (P33) will be occur.
(10) If the usage data count valid signal (YC8A) is ON, G10 L3 or G10 L30 cannot be commanded. (11) The registered data is held even if the power is turned OFF. (12) When G10 L3 or G10 L30 is commanded, the commanded group and tool will be registered
after all of the registered data is erased. (13) The change and addition conditions in the G10L3P1 or G10 L30 P1 command are as follows.
(a) Change conditions Both the commanded group No. and tool No. are registered. Change the commanded tool No. data.
(b) Additional conditions Neither the commanded group No. nor tool No. is registered. Additionally register the commanded group No. and tool No. data.
The commanded group No. is registered, but the commanded tool No. is not registered. Additionally register the commanded tool No. data to the commanded group No.
(14) The setting range of the tool compensation No. will differ according to the specifications (number of tool compensation sets).
Relation with other functions
(1) During the following operations, the tool usage data will not be counted.
Machine lock Miscellaneous function lock Dry run Single block Skip
13. Program Support Functions 13.1 Fixed Cycles
247
13. Program Support Functions 13.1 Fixed Cycles 13.1.1 Standard Fixed Cycles; G80 to G89, G73, G74, G75, G76
Function and purpose
These standard canned cycles are used for predetermined sequences of machining operations such as positioning, hole drilling, boring, tapping, etc. which are specified in a block. The various sequences in the table below are provided for the standard canned cycles. By editing the standard canned cycle subprogram, the canned cycle sequence can be changed by the user. The user can also register and edit an original canned cycle program. For the standard canned cycle subprogram, refer to the list of the canned cycle subprogram in the appendix of the operation manual. The list of canned cycle functions for this control unit is shown below.
Operation at hole bottom G code
Hole machining start
(-Z direction) Dwell Spindle
Return operation
(+Z direction)
Retract at high- speed
Application
G80 — — — — — Cancel
G81 Cutting feed — — Rapid feed Available Drill, spot drilling cycle
G82 Cutting feed Yes — Rapid feed — Drill, counter boring cycle
G83 Intermittent feed — — Rapid feed Available Deep hole drilling cycle
G84 Cutting feed Yes Reverse rotation Cutting feed — Tapping cycle
G85 Cutting feed — — Cutting feed — Boring cycle
G86 Cutting feed Yes Stop Rapid feed — Boring cycle
G87 Cutting feed — Forward rotation Cutting feed — Back boring
cycle
G88 Rapid traverse Yes Stop Rapid feed — Boring cycle
G89 Cutting feed Yes — Cutting feed — Boring cycle
G73 Cutting feed Yes — Rapid feed Available Stepping cycle
G74 Intermittent feed Yes Forward rotation Cutting feed — Reverse tapping
cycle
G75 Cutting feed — — Rapid feed — Circular cutting cycle
G76 Cutting feed — Oriented spindle stop Rapid feed — Fine boring
cycle
A canned cycle mode is canceled when the G80 or any G command in (G00, G01, G02, G03) is issued. The various data will also be cleared simultaneously to zero.
13. Program Support Functions 13.1 Fixed Cycles
248
Command format
G8 (G7) X__ Y__ Z__ R__ Q__ P__ F__ L__ S__ , S __ ,I__ ,J__; G8 (G7) X__ Y__ Z__ R__ Q__ P__ F__ L__ S__ , R __ ,I__ ,J__; G8 (G7): Hole machining mode X Y Z R Q P F L S , S
: Hole positioning data : Hole machining data : Number of repetitions (When «0» is set, drilling is not executed at a command block.)
: Spindle rotation speed : Spindle rotation speed during retraction
, R , I , J
: Synchronization changeover : Positioning axis in-position width : Drilling axis in-position width
As shown above, the format is divided into the hole machining mode, hole positioning data, hole machining data, No. of repetitions, spindle rotation speed, synchronization changeover (or spindle rotation speed during return), positioning axis in-position width and drilling axis in-position width.
Detailed description
(1) Outline of data and corresponding addresses
(a) Hole machining mode: Canned cycle modes such as drilling, counter boring, tapping and boring.
(b) Hole position data: Data used to position the X and Y axes. (Unmodal) (c) Hole machining data: Actual machining data used for machining. (Modal) (d) Number of repetitions: Number of times to carry out hole machining. (Unmodal) (e) Synchronization changeover: Synchronous/asynchronous tapping selection command is
issued during G84/G74 tapping. (Modal)
(2) If M00 or M01 is commanded in the same block as the canned cycle or during the canned cycle mode, the canned cycle will be ignored. Instead, M00 and M01 will be output after positioning. The canned cycle will be executed if X, Y, Z or R is commanded.
13. Program Support Functions 13.1 Fixed Cycles
249
(3) There are 7 actual operations which are each described in turn below.
Operation 1
R point
Initial point Operation 2
Operation 3
Operation 4
Operation 5
Operation 6
Operation 7
Operation 1 : This indicates the X and Y axes positioning, and executes positioning with G00. Operation 2 : This is an operation done after positioning is completed (at the initial hole), and
when G87 is commanded, the M10 command is output from the control unit to the machine. When this M command is executed and the finish signal (FIN) is received by the control unit, the next operation will start. If the single block stop switch is ON, the block will stop after positioning.
Operation 3 : The tool is positioned to the R point by rapid traverse. Operation 4 : Hole machining is conducted by cutting feed. Operation 5 : This operation takes place at the hole bottom position and it differs according to
the canned cycle mode. Possible actions include spindle stop (M05) spindle reverse rotation (M04), spindle forward rotation (M03), dwell and tool shift.
Operation 6 : The tool is retracted to the R point. Operation 7 : The tool is returned to the initial pint at the rapid traverse rate. Whether the canned cycle is to be completed at operation 6 or 7 can be selected by the following G commands. G98 ………… Initial level return G99 ………… R point level return These are modal commands, and for example, if G98 is commanded once, the G98 mode will be entered until G99 is designated. The initial state when the NC is ready is the G98 mode. The hole machining data will be ignored if X, Y, Z or R is not commanded. This function is mainly used with the special canned cycled.
(4) Canned cycle addresses and meanings
Address Significance G Selection of hole machining cycle sequence (G80 to G89, G73, G74, G76) X Designation of hole drilling position (absolute value or incremental value) Y Designation of hole drilling position (absolute value or incremental value) Z Designation of hole bottom position (absolute value or incremental value)
P Designation of dwell time at hole bottom position (decimal points will be ignored) or designation of tool radius compensation No. for G75
Q Designation of cut amount for each cutting pass for G73 or G83, designation of the shift amount for G76 or G87 (incremental value), or designation of the radius of outer circumference for G76 or G87
R Designation of R point position (absolute value or incremental value)
F Designation of feed rate for cutting feed (asynchronous tapping) or number of Z axis pitch (synchronous tapping)
L Designation of number of repetitions. (0 to 9999) When 0 is set, no execution
I, J, K Designation of shift amount for G76 or G87 (incremental value) (The shift amount is designated with Q address according to the parameter setting.)
13. Program Support Functions 13.1 Fixed Cycles
250
Address Significance
S
Spindle rotation speed command (Note1) S command that was issued with the form of Sn = ****** will be
ignored during the synchronous tapping. (n:spindle No., *****:rotation speed)
(Note2) If S command is issued in the synchronous tapping modal, the program error (P186) will occur.
,S Spindle rotation speed designation during retraction
,R Designation of synchronous tapping/asynchronous tapping (If «,R» setting is omitted, that depends on the parameter setting.)
M
Designation of miscellaneous command (Note) On the asynchronous tapping with normal tapping, spindle forward
rotation will be applied for Mm1 basically. Note that the spindle reverse rotation should be commanded with M(m1 + 1), that is, the M code of spindle forward rotation command +1, or that could lead an incorrect operation.
,I Designation of positioning axis in-position width ,J Designation of drilling axis in-position width
(5) Difference between absolute value command and incremental value command
For absolute value
R point +r
-r
-z
-z
For incremental value
Workpiece Workpiece
R point
(6) Feed rate for tapping cycle and tapping return The feed rates for the tapping cycle and tapping return are as shown below. (a) Selection of synchronous tapping cycle/asynchronous tapping cycle
Program G84, Rxx Control parameter Synchronous tapping
Synchronous/ asynchronous
, R00 OFF
Asynchronous , Rxx
No designation ON , R01
Synchronous
is irrelevant to the setting
13. Program Support Functions 13.1 Fixed Cycles
251
(b) Selection of asynchronous tapping cycle feed rate
G94/G95 Control parameter F1-digit value F command value Feed designation
OFF F designation Other than F0 to F8
Per-minute feed G94
ON F0 to F8 (no decimal point) F1-digit feed
G95 F designation Per-revolution feed is irrelevant to the setting
(c) Spindle rotation speed during return of synchronous tapping cycle
Address Meaning of address
Command range (unit) Remarks
,S Spindle rotation speed during return
0 to 99999 (r/min)
The data is held as modal information. If the value is smaller than the speed rotation speed, the speed rotation speed value will be valid even during return. If the spindle rotation speed is not 0 during return, the tap return override value will be invalid.
(7) M code for forward/reverse rotation command.
The M code set with the parameter #3028 sprcmn is output as the M code for spindle forward/reverse rotation that is output at hole bottom or at R point during asynchronous tapping cycle. Note that the M code for forward rotation is output as M3 and that for reverse rotation is as M4 if the parameter #3208) is set to 0.
Positioning plane and hole drilling axis
The canned cycle has basic control elements for the positioning plane and hole drilling axis. The positioning plane is determined by the G17, G18 and G19 plane selection command, and the hole drilling axis is the axis perpendicular (X, Y, Z or parallel axis) to the above plane.
Plane selection Positioning plane Hole drilling axis G17 (X Y) Xp Yp Zp G18 (Z X) Zp Xp Yp G19 (Y Z) Yp Zp Xp
Xp, Yp and Zp indicate the basic axes X, Y and Z or an axis parallel to the basic axis. A random axis other than the hole drilling axis can be commanded for positioning. The hole drilling axis is determined by the axis address of the hole drilling axis commanded in the same block as G81 to G89, G73, G74 or G76. The basic axis will be the hole drilling axis if there is no designation.
(Example1) When G17 (XY plane) is selected, and the axis parallel to the Z axis is set as the W
axis. G81 … W__; The W axis is used as the hole drilling axis. G81 … Z __; The Z axis is used as the hole drilling axis. G81 … ; (No Z or W) The Z axis is used as the hole drilling axis.
(Note 1) The hole drilling axis can be fixed to the Z axis with parameter #1080 Dril_Z. (Note 2) Change over the hole drilling axis in the canned cycle canceled state.
In the following explanations on the movement in each canned cycle mode, the XY plane is used for the positioning plane and the Z axis for the hole drilling axis. Note that all command values will be incremental values, the positioning plane will be the XY plane and the hole drilling axis will be the Z axis.
13. Program Support Functions 13.1 Fixed Cycles
252
Programmable in-position width command in fixed cycle
This command commands the in-position width for the fixed cycle from the machining program. The commanded in-position width is valid only in the G81 (drill, spot drill), G82 (drill, counter boring), G83 (deep drill cycle), G84 (tap cycle), G85 (boring), G89 (boring), G73 (step cycle) and G74 (reverse tap cycle) fixed cycles. The «, I» address is commanded in respect to the positioning axis, and the «,J» address is commanded in respect to the drilling axis.
Address Meaning of address Command range (unit) Remarks
,I In-position width (position error amount)
,J In-position width for drilling axis in fixed cycle (position error amount)
0.001 to 999.999 (mm)
When a value exceeding the command range is issued, a program error will occur. (P35)
In-position check in fixed cycle
When the number of repetitions L is designated as two or more times in the fixed cycle, the commanded in-position width will be valid in the repetition block (operation 5 to operation 8). : G81 X-50. Z-50. R-50. L2 F2000, I0.2, J0.3 ; :
Operation1 -50.
Operation5
Operation2
Operation3 Operation4
Operation7 Operation8
Operation6
-50.
Fig. 1 Operation when number of repetitions L is designated
In the following machining program, the commanded in-position width is valid for the Fig. 2 block. In the (B) block, the in-position width (, I) commanded for positioning in the previous block (A) is invalid (operation 5). However, when returning from the hole bottom, the in-position width (, J) commanded in the previous block (A) is valid (operation 8). To validate the in-position width for positioning, command again as shown in block (C) (Operation 9). : G81 X-50. Z-50. R-50. F2000, I0.2, J0.3 ;……..(A) X-10. ; …………………………………………………………..(B) X-10., I0.2 ; ……………………………………………………(C) :
Operation pattern ,I ,J
Operation 1 Valid Operation 2 Invalid Operation 3 Invalid Operation 4 Valid Operation 5 Valid Operation 6 Invalid Operation 7 Invalid Operation 8 Valid
13. Program Support Functions 13.1 Fixed Cycles
253
Operation1
Operation4
Opera- tion7
Opera- tion6
Operation5 -10.
Opera-
tion12 Operation8
Opera- tion11
Opera- tion10
Operation9 -10.
Operation2
Operation3
-50.
Operation pattern
,I ,J
Operation 1 Valid Operation 2 Invalid Operation 3 Invalid Operation 4 Valid Operation 5 Invalid Operation 6 Invalid Operation 7 Invalid Operation 8 Valid Operation 9 Valid Operation 10 Invalid Operation 11 Invalid Operation 12 Valid
Fig. 2 Operation in fixed cycle modal
Setting values of synchronous tap in-position check parameters and tap axis movement
(1) Synchronous tap in-position check settings
#1223 aux07 Bit3 Bit4 Bit5 Bit2
Synchronous tapping
in-position check
At hole bottom
At R point
I point R point
«P» designation of G84/G74 command
In-position check during synchronous tapping
0 Carry out in-position check at I point R point/R point/hole bottom.
1 No «P» designation
Example: G84 F1. Z-5. S1000 R-5.
Hole bottom: R point:
I point R point:
Do not carry out in-position check. Do not carry out in-position check. Do not carry out in-position check.
1 1 1 1 «P» designation
Example: G84 F1. Z-5. S1000 PO R-5.
Hole bottom:
R point: I point R point:
Carry out in-position check by tap in-position width. Carry out in-position check. Carry out in-position check.
1 1 0 1 «P» designation
Example: G84 F1. Z-5. S1000 PO R-5.
Hole bottom:
R point: I point R point:
Carry out in-position check by tap in-position width. Do not carry out in-position check. Carry out in-position check.
1 0 1 1 «P» designation
Example: G84 F1. Z-5. S1000 PO R-5.
Hole bottom: R point:
I point R point:
Do not carry out in-position check. Carry out in-position check. Carry out in-position check.
1 0 0 1 «P» designation
Example: G84 F1. Z-5. S1000 PO R-5.
Hole bottom: R point:
I point R point:
Do not carry out in-position check. Do not carry out in-position check. Carry out in-position check.
1 1 1 0 «P» designation
Example: G84 F1. Z-5. S1000 PO R-5.
Hole bottom:
R point: I point R point:
Carry out in-position check by tap in-position width. Carry out in-position check. Do not carry out in-position check.
1 1 0 0 «P» designation
Example: G84 F1. Z-5. S1000 PO R-5.
Hole bottom:
R point: I point R point:
Carry out in-position check by tap in-position width. Do not carry out in-position check. Do not carry out in-position check.
1 0 1 0 «P» designation
Example: G84 F1. Z-5. S1000 PO R-5.
Hole bottom: R point:
I point R point:
Do not carry out in-position check. Carry out in-position check. Do not carry out in-position check.
1 0 0 0 «P» designation
Example: G84 F1. Z-5. S1000 PO R-5.
Hole bottom: R point:
I point R point:
Do not carry out in-position check. Do not carry out in-position check. Do not carry out in-position check.
(Note 1) The I point refers to the initial point.
13. Program Support Functions 13.1 Fixed Cycles
254
(2) Relation between the in-position width and tap axis movement for a synchronous tap
in-position check
Time T
Speed
Hole bottom
FIN R point
(2)(4) (3) (1)
In-position completion of the G0 feed from the R point
G1 deceleration start at tap return
Start of G0 feed to the R point G1
deceleration start at tap cut-in
R point : In-position check by the G1inps value. I point : In-position check by the G0inps value. Hole bottom : In-position check by the Tapinps value.
(1) Section in which the in- position check is carried out by the sv024 value.
(2) Section in which the in- position check is carried out by the TapInp value.
(3) Section in which the in- position check is carried out by the G1inps value.
(4) Section in which the in- position check is carried out by the G0inps value.
13. Program Support Functions 13.1 Fixed Cycles
255
(3) Relation between the parameter setting values and tap axis movement for a synchronous tap in-position check
#1223 aux07 Bit3 Bit4 Bit5 Bit2
Synchronous tapping
in-position check
At hole bottom
At R point
At I point R point
Hole bottom wait time
Operation at hole bottom
Operation at R point
Operation at I point R point
0
Time designated by «P». Processing time is several 10ms when no «P».
Operation determined by setting of inpos (#1193) and aux 07 (#1223): bit 1 parameters.
Operation determined by setting of inpos (#1193) and aux 07 (#1223): bit 1 parameters.
Operation determined by setting of inpos (#1193) and aux 07 (#1223): bit 1 parameters.
1 0 0 1
Larger value of «P» and TapDwl (#1313) is valid. No dwell executed if both values are 0.
Wait until time in left column has elapsed.
Wait until completion of in-position check by G0inps value.
1 0 1 1
Larger value of «P» and TapDwl (#1313) is valid. No dwell executed if both values are 0.
Wait until time in left column has elapsed.
Wait until completion of in-position check by G1inps value.
Wait until completion of in-position check by G0inps value.
1 1 0 1
Larger value of «P» and TapDwl (#1313) is valid. No dwell executed if both values are 0.
Wait until dwell time in left column has elapsed after completion of in-position check.
Wait until completion of in-position check by G0inps value.
1 1 1 1
Larger value of «P» and TapDwl (#1313) is valid. Processing time is several 10ms if both values are 0.
Wait until dwell time in left column has elapsed after completion of in-position check.
Wait until completion of in-position check by G1inps value.
Wait until completion of in-position check by G0inps value.
1 0 0 0 Larger value of «P» and TapDwl (#1313) is valid. No dwell executed if both values are 0.
Wait until time in left column has elapsed.
1 0 1 0
Larger value of «P» and TapDwl (#1313) is valid. No dwell executed if both values are 0.
Wait until time in left column has elapsed.
Wait until completion of in-position check by G1inps value.
1 1 0 0
Larger value of «P» and TapDwl (#1313) is valid. No dwell executed if both values are 0.
Wait until dwell time in left column has elapsed after completion of in-position check.
1 1 1 0
Larger value of «P» and TapDwl (#1313) is valid. Processing time is several 10ms if both values are 0.
Wait until dwell time in left column has elapsed after completion of in-position check.
Wait until completion of in-position check by G1inps value.
(Note 1) The I point refers to the initial point. Remarks: The processing time is several 10ms when an in-position check is not carried out at the hole bottom.
The processing time is between 0 to 14.2ms when an in-position check is not carried out at the R point. The processing time is the spindle gain changeover time when an in-position check is not carried out at I point R point.
13. Program Support Functions 13.1 Fixed Cycles
256
Movement when executing each fixed cycles
(a) G81 (Drilling, spot drilling)
Program G81 Xx1 Yy1 Zz1 Rr1 Ff1 ,Ii1 ,Jj1;
(1) G0 Xx1 Yy1 (2) G0 Zr1 (3) G1 Zz1 Ff1 (4) G98 mode G0Z (z1+r1) G99 mode G0Z z1
G98 G99 mode mode
(1)
(2)
(3) (4)
x1 , y1
z1
r1
(4)
The operation stops at after the (1), (2) and (4) commands during single block operation.
Operation pattern i1 j1
(1) Valid — (2) — Invalid (3) — Invalid (4) — Valid
(b) G82 (Drilling, counter boring)
Program G82 Xx1 Yy1 Zz1 Rf1 Ff1 Pp1 ,Ii1 ,Jj1; P : Dwell designation
(1) G0 Xx1 Yy1 (2) G0 Zr1 (3) G1 Zz1 Ff1 (4) G4 Pp1 (Dwell) (5) G98 mode G0Z (z1+r1) G99 mode G0Z z1
G98 G99 mode mode
(1) x1 , y1
z1
r1(2)
(3)
(4)
(5) (5)
Operation pattern i1 j1
(1) Valid — (2) — Invalid (3) — Invalid (4) — — (5) — Valid
The operation stops at after the (1), (2) and (5) commands during single block operation.
13. Program Support Functions 13.1 Fixed Cycles
257
(c) G83 (Deep hole drilling cycle)
Program G83 Xx1 Yy1 Zz1 Rr1 Qq1 Ff1 ,Ii1 ,Jj1; Q : This designates the cutting amount per pass, and is always designated with an
incremental value.
(1) G0 Xx1 Yy1 (2) G0 Zr1 (3) G1 Zq1 Ff1 (4) G0 Z q1 (5) G0 Z (q1 m) (6) G1 Z (q1 + m) Ff1 (7) G0 Z 2 q1 (8) G0 Z (2 q1 m) (9) G1 Z (q1 + m) Ff1 (10) G0 Z 3 q1
: :
(n) G98 mode G0Z (z1+r1) G99 mode G0Z z1
G98 G99 mode mode
(1)
(n)
(n) — 1
x1,y1
q1
q1
q1
r1
z1
m
m
(3) (4) (5)
(6) (7) (8)
(9)
(10)
(2)
(n)
Operation
pattern i1 j1
(1) Valid — (2) — Invalid (3) — Invalid (4) — Invalid (5) — Invalid (6) — Invalid (7) — Invalid (8) — Invalid (9) — Invalid (10) — Invalid
: :
n-1 — Invalid n — Valid
When executing a second and following cutting in the G83 as shown above, the movement will change from rapid traverse to cutting feed several mm (m mm in the figure above) before the position machined last. When the hole bottom is reached, the axis will return according to the G98 or G99 mode. m will differ according to the parameter «#8013 G83 return». Program so that q1>m. The operation stops at after the (1), (2) and n commands during single block operation.
13. Program Support Functions 13.1 Fixed Cycles
258
(d) G84 (Tapping cycle)
Program G84 Xx1 Yy1 Zz1 Rr1 Ff1 Pp1 Rr2 (or S1, S2) ,Ii1 ,Jj1; P : Dwell designation
(1) G0 Xx1 Yy1 (2) G0 Zr1 (3) G1 Zz1 Ff1 (4) G4 Pp1 (5) M4 (Spindle reverse rotation) (6) G1 Z z1 Ff1 (7) G4 Pp1 (8) M3 (Spindle forward rotation) G98 mode G0Z r1 G99 mode No movement
G98 G99 mode mode
(4) (5)
r1
z1
(1) x1 ,y1
(2)
(3) (6)
(7) (8)
(9) (6)
(7) (8)
Operation
pattern i1 j1
(1) Valid — (2) — Invalid (3) — Invalid (4) — — (5) — — (6) — Invalid (7) — — (8) — — (9) — Valid
When r2 = 1, the synchronous tapping mode will be entered, and when r2 = 0, the
asynchronous tapping mode will be entered. When G84 is executed, the override will be canceled and the override will automatically
be set to 100%. Dry run is valid when the control parameter «G00 DRY RUN» is on and is valid for the
positioning command. If the feed hold button is pressed during G84 execution, and the sequence is at (3) to (6), the movement will not stop immediately, and instead will stop after (6). During the rapid traverse in sequence (1), (2) and (9), the movement will stop immediately.
The operation stops at after the (1), (2) and (9) commands during single block operation. During the G84 modal, the «Tapping» NC output signal will be output. During the G84 synchronous tapping modal, the M3, M4, M5 and S code will not be
output.
13. Program Support Functions 13.1 Fixed Cycles
259
This function allows spindle acceleration/deceleration pattern to be approached to the speed loop acceleration/deceleration pattern by dividing the spindle and drilling axis acceleration/deceleration pattern into up to three stages during synchronous tapping. The acceleration/deceleration pattern can be set up to three stages for each gear. When returning from the hole bottom, rapid return is possible depending on the spindle rotation speed during return. The spindle rotation speed during return is held as modal information. (i) When tap rotation speed < spindle rotation speed during return synchronous tap changeover spindle rotation speed 2
Smax S2
S(S1)
S1 S’ S2
Smax
T1
T1 T1
T1
T2
T2
S : Command spindle rotation speed S’ : Spindle rotation speed during return S1 : Tap rotation speed (spindle base specification parameters #3013 to #3016) S2 : Synchronous tap changeover spindle rotation speed 2
(spindle base specification parameters #3037 to #3040) Smax : Maximum rotation speed (spindle base specification parameters #3005 to
#3008) T1 : Tap time constant (spindle base specification parameters #3017 to #3020) T2 : Synchronous tap changeover time constant 2
(spindle base specification parameters #3041 to #3044)
13. Program Support Functions 13.1 Fixed Cycles
260
(ii) When synchronous tap changeover spindle rotation speed 2 < spindle rotation speed during return
Smax S2 S(S1)
S1 S2
S'(Smax)
T1
T2 T1T1
T1
T2
T3
T3
S : Command spindle rotation speed S’ : Spindle rotation speed during return S1 : Tap rotation speed (spindle base specification parameters #3013 to #3016) S2 : Synchronous tap changeover spindle rotation speed 2
(spindle base specification parameters #3037 to #3040) Smax : Maximum rotation speed (spindle base specification parameters #3005 to
#3008) T1 : Tap time constant (spindle base specification parameters #3017 to #3020) T2 : Synchronous tap changeover time constant 2
(spindle base specification parameters #3041 to #3044) T3 : Synchronous tap changeover time constant 3
(spindle base specification parameters #3045 to #3048)
13. Program Support Functions 13.1 Fixed Cycles
261
(iii) Pecking tapping cycle
The load applied to the tool can be reduced by designating the depth of cut per pass (Q) and cutting the workpiece to the hole bottom for a multiple number of passes. The amount retracted from the hole bottom is set to the parameter «#8018 G84/G74 return». Select either the pecking tapping cycle or the deep-hole tapping cycle by parameter. («#1272 ext08/bit4») When «depth of cut per pass Q» is designated in the block containing the G84 or G74 command in the state where the pecking tapping cycle is selected, the pecking tapping cycle is executed. In the following cases, the normal tapping cycle is established.
When Q is not designated When the command value of Q is zero
G84 Xx1 Yy1 Zz1 Rr1 Qq1 Ff1 Ee1 Pp1 Ss1 ,Ss2 ,Ii1 ,Jj1 ,Rr2 ;
X, Yy Z R Q F E P S , S , I , J , R
: Hole drilling position : Hole bottom position : Point R position : Depth of cut per pass (designated as an incremental position) : Z-axis feed amount (tapping pitch) per spindle rotation : Tap thread number per 1-inch feed of Z axis : Dwell time at hole bottom position : Rotation speed of spindle : Rotation speed of spindle during retract : In-position width of positioning axis : In-position width of hole drilling axis : Synchronization method selection (r2=1 synchronous, r2=0 asynchronous)
(Note) When «,R0» is commanded, F address is regarded as cutting federate. Refer to the section «Fixed cycle» for details.
q1
m
m q1
q1
r1
z1
x1, y1
(1)
(2)
(3) (6)
(4) (5) (7)
(10)
(9) (11)(8)
(n7)
(n5) (n6) (n5) (n6)
(n4) (n4)
(n1)
(n2) (n3) M98 mode
M99 mode
(1) G0 Xx1 Yy1 , Ii1 (2) G0 Zr1 (3) G1 Zq1 Ff1 (4) M4 (Spindle reverse rotation) (5) G1 Z-m Ff1 (6) M3 (Spindle forward rotation) (7) G1 Z(q1+m) Ff1 (8) M4 (Spindle reverse rotation) (9) G1 Z-m Ff1 (10) M3 (Spindle forward rotation) (11) G1 Z(q1+m) Ff1 : : (n1) G1 Z(z1-q1*n) Ff1 (n2) G4 Pp1 (n3) M4 (Spindle reverse rotation) (n4) G1 Z-z1 Ff1 Ss2 (n5) G4 Pp1 (n6) M3 (Spindle forward rotation) G98 mode G0 Z-r1 , Ij1 G99 mode No movement
(n7)
* 1. m: Parameter «#8018 G84/G74 return» 2. This program is for the G84 command. The spindle forward rotation (M3)
and reverse rotation (M4) are reversed with the G74 command.
13. Program Support Functions 13.1 Fixed Cycles
262
(iv) Deep-hole tapping cycle
In the deep-hole tapping, the load applied to the tool can be reduced by designating the depth of cut per pass and cutting the workpiece to the hole bottom for a multiple number of passes. Under the deep-hole tapping cycle, the tool is retracted to the R-point every time. Select either the pecking tapping cycle or the deep-hole tapping cycle by parameter. («#1272 ext08/bit4») When «depth of cut per pass Q» is designated in the block containing the G84 or G74 command in the state where the deep-hole tapping cycle is selected by parameter, the deep-hole tapping cycle is executed. In the following cases, the normal tapping cycle is established. When Q is not designated When the command value of Q is zero
G84 Xx1 Yy1 Zz1 Rr1 Qq1 Ff1 Ee1 Pp1 Ss1 ,Ss2 ,Ii ,Jj ,Rr2 ;
X,Y Z R Q F E P S ,S ,I ,J ,R
: Hole drilling position : Hole bottom position : Point R position : Depth of cut per pass (designated as an incremental position) : Z-axis feed amount (tapping pitch) per spindle rotation : Tap thread number per 1-inch feed of Z axis : Dwell time at hole bottom and point R return : Rotation speed of spindle : Rotation speed of spindle during retract : In-position width of positioning axis : In-position width of hole drilling axis : Synchronization method selection (r2=1 synchronous, r2=0 asynchronous)
(Note) When «,R0» is commanded, F address is regarded as cutting federate. Refer to the section «Fixed cycle» for details.
(1)
r1
z1
G98 mode
G99 mode
q1
x1,y1
R point
q1
q1
(2)
(3)
(4)
(5)
(6)(7)
(8)
(10)
(13)
(11)(12)
(9)
(n7)
(n5)(n6)
(n1) (n4) (n4)
(n2)(n3)
(n5)(n6)
(1) G0 Xx1 Yy1 (2) G0 Zr1 (3) G9 G1 Zq1 Ff1 (4) M4 (Spindle reverse rotation) (5) G9 G1 Z-q1 Ff1 (6) G4 Pp1 (7) M3 (Spindle forward rotation) (8) G9 G1 Z(2?q1) Ff1 (9) M4 (Spindle reverse rotation) (10) G9 G1 Z-(2?q1) Ff1 (11) G4 Pp1 (12) M3 (Spindle forward rotation) (13) G9 G1 Z(3?q1) Ff1
: (n1) G9 G1 Zz1 Ff1 (n2) G4 Pp1 (n3) M4 (Spindle reverse rotation) (n4) G9 G1 Z-z1 Ff1 (n5) G4 Pp1 (n6) M3 (Spindle forward rotation) (n7) G98 mode G0 Z-r1 G99 mode No movement
*1. This program is for the G84 command. The spindle forward rotation (M3) and reverse rotation (M4) are reversed with the G74 command.
13. Program Support Functions 13.1 Fixed Cycles
263
(e) G85 (Boring)
Program G85 Xx1 Yy1 Zz1 Rr1 Ff1 ,Ii1 ,Jj1;
(1) G0 Xx1 Yy1 (2) G0 Zr1 (3) G1 Zz1 Ff1 (4) G1 Z z1 Ff1 G98 mode G0Z r1 G99 mode No movement
G98 G99 mode mode
r1
z1
(1) x1 , y1
(2)
(3)
(5)
(4) (4)
(5)
Operation pattern i1 j1
(1) Valid — (2) — Invalid (3) — Invalid (4) — Invalid (5) — Valid
The operation stops at after the (1), (2), and (4) or (5) commands during single block operation.
(f) G86 (Boring)
Program G86 Xx1 Yy1 Zz1 Rr1 Ff1 Pp1 ;
G98 G99 mode mode
(4)(5)
(1) x1 , y1
z1
r1(2)
(3) (6) (6)
(7)
(1) G0 Xx1 Yy1 (2) G0 Zr1 (3) G1 Zz1 Ff1 (4) G4 Pp1 (5) M5 (Spindle stop) G98 mode G0Z (z1+r1) G99 mode G0Z z1 (7) M3 (Spindle forward rotation)
(7)
(6)
The operation stops at after the (1), (2) and (7) commands during single block operation.
13. Program Support Functions 13.1 Fixed Cycles
264
(g) G87 (Back boring)
Program G87 Xx1 Yy1 Zz1 Rr1 Iq1 Jq2 Ff1 ; (Note) Take care to the z1 and r1 designations. (The z1 and r1 symbols are reversed). There is no R point return.
(1)
r1
Xq1(Yq2)
(12)(11)
z1
x1 , y1
(2)
(8) (9)
(7)
(6) (5)
(4)
(10)
(3) (1) G0 Xx1 Yy1 (2) M19 (Spindle orient) (3) G0 Xq1 (Yq2) (Shift) (4) G0 Zr1 (5) G1 Xq1 (Yq2) Ff1 (Shift) (6) M3 (Spindle forward rotation) (7) G1 Zz1 Ff1 (8) M19 (Spindle orient) (9) G0 Xq1 (Yq2) (Shift) G98 mode G0Z (z1+r1) G99 mode G0Z (r1+z1) (11) G0 Xq1 (Yq2) (Shift) (12) M3 (Spindle forward rotation)
(10)
The operation stops at after the (1), (4), (6) and (11) commands during single block operation. When this command is used, high precision drilling machining that does not scratch the machining surface can be done. (Positioning to the hole bottom and the escape (return) after cutting is executed in the state shifted to the direction opposite of the cutter.) The shift amount is designated as shown below with addresses I, J and K.
Spindle orient position
Cutter
Tool during cutting Tool after cutting
Cancel
Shift
Machining hole
Cancel
Shift
Shift amount
The shift amount is executed with linear interpolation, and the feed rate follows the F command. Command I, J, and K with incremental values in the same block as the hole position data. I, J and K will be handled as modals during the canned cycle. (Note) If the parameter «#1080 Dril_Z» which fixes the hole drilling axis to the Z axis is
set, the shift amount can be designated with address Q instead of I and j. In this case, whether to shift or not and the shift direction are set with parameter «#8207 G76/87 No shift» and «#8208 G76/87 Shift ()». The symbol for the Q value is ignored and the value is handled as a positive value.
The Q value is a modal during the canned cycle, and will also be used as the G83, G73 and G76 cutting amount.
For G17 : I, J For G18 : K, I For G19 : J, K
13. Program Support Functions 13.1 Fixed Cycles
265
(h) G88 (Boring)
Program G88 Xx1 Yy1 Zz1 Rr1 Ff1 Pp1 ;
(1) G0 Xx1 Yy1 (2) G0 Zr1 (3) G1 Zz1 Ff1 (4) G4 Pp1 (5) M5 (Spindle stop) (6) Stop when single block stop
switch is ON. (7) Automatic start switch ON G98 mode G0Z (z1+r1) G99 mode G0Z z1 (9) M3 (Spindle forward rotation)G98 G99
mode mode (4)(5)(6)(7)
(1) x1 , y1
z1
r1 (2)
(3) (8) (8)
(9)
(9)
(8)
The operation stops at after the (1), (2), (6) and (9) commands during single block operation.
(i) G89 (Boring)
Program G89 Xx1 Yy1 Zz1 Rr1 Ff1 Pp1, Ii1, Jj1;
(1) G0 Xx1 Yy1 (2) G0 Zr1 (3) G1 Zz1 Ff1 (4) G4 Pp1 (5) G1 Z z1 Ff1 G98 mode G0Z r1 G99 mode No movement
G98 G99 mode mode
r1
z1
(1)
(6)
x1 , y1
(2)
(3)
(4)
(5) (5) (6)
Operation pattern i1 j1
(1) Valid — (2) — Invalid (3) — Invalid (4) — — (5) — Invalid (6) — Valid
The operation stops at after the (1), (2) and (5) or (6) commands during single block operation.
13. Program Support Functions 13.1 Fixed Cycles
266
(j) G73 (Step cycle)
Program G73 Xx1 Yy1 Zz1 Qq1 Rr1 Ff1 Pp1 ,Ii1 ,Jj1; P : Dwell designation
G98 G99 mode mode
(1) G0 Xx1 Yy1 (2) G0 Zr1 (3) G1 Zq1 Ff1 (4) G4 Pp1 (5) G0 Z m (6) G1 Z (q1 + m) Ff1 : (n) G98 mode G0Z (z1+r1) G99 mode G0Z z1
(1)
(3)
x1 , y1
z1
r1
q
q
q
(n) m
(n) -1
(2)
(4) (5) (6)
(n)
Operation
pattern i1 j1
(1) Valid — (2) — Invalid (3) — Invalid (4) — — (5) — Invalid (6) — Invalid
: :
(n) -1 — Invalid
(n) — Valid
When executing a second and following cutting in the G73 as shown above, the movement will return several mm (m mm in the figure above) with rapid traverse and then will change to cutting feed. The return amount m will differ according to the parameter «#8012 G73 return». The operation stops at after the (1), (2) and (n) commands during single block operation.
13. Program Support Functions 13.1 Fixed Cycles
267
(k) G74 (Reverse tapping cycle)
Program G74 Xx1 Yy1 Zz1 Rr1 Pp1 Rr2(or S1,S2) ,Ii1 ,Jj1; P : Dwell designation
(1) G0 Xx1 Yy1 (2) G0 Zr1 (3) G1 Zz1 Ff1 (4) G4 Pp1 (5) M3 (Spindle forward rotation) (6) G1 Z z1 Ff1 (7) G4 Pp1 (8) M4 (Spindle reverse rotation) G98 mode G0Z r1 G99 mode No movement
G98 G99 mode mode(4)(5)
r1
z1
(1) x1 ,y1
(7)(8) (2)
(3)
(7) (8) (9)
(6) (6)
(9)
Operation
pattern i1 j1
(1) Valid — (2) — Invalid (3) — Invalid (4) — — (5) — — (6) — Invalid (7) — — (8) — — (9) — Valid
When r2 = 1, the synchronous tapping mode will be entered, and when r2 = 0, the asynchronous tapping mode will be entered. When G74 is executed, the override will be canceled and the override will automatically be set to 100%. Dry run is valid when the control parameter «#1085 G00Drn» is set to «1» and is valid for the positioning command. If the feed hold button is pressed during G74 execution, and the sequence is at (3) to (6), the movement will not stop immediately, and instead will stop after (6). During the rapid traverse in sequence (1), (2) and (9), the movement will stop immediately. The operation stops at after the (1), (2) and (9) commands during single block operation. During the G74 and G84 modal, the «Tapping» NC output signal will be output. During the G74 synchronous tapping modal, the M3, M4, M5 and S code will not be output.
13. Program Support Functions 13.1 Fixed Cycles
268
This function allows spindle acceleration/deceleration pattern to be approached to the speed loop acceleration/deceleration pattern by dividing the spindle and drilling axis acceleration/deceleration pattern into up to three stages during synchronous tapping. The acceleration/deceleration pattern can be set up to three stages for each gear. When returning from the hole bottom, rapid return is possible depending on the spindle rotation speed during return. The spindle rotation speed during return is held as modal information. (i) When tap rotation speed < spindle rotation speed during return synchronous tap changeover spindle rotation speed 2
Smax S2
S(S1)
S1 S’ S2
Smax
T1
T1 T1
T1
T2
T2
S : Command spindle rotation speed S’ : Spindle rotation speed during return S1 : Tap rotation speed (spindle base specification parameters #3013 to #3016) S2 : Synchronous tap changeover spindle rotation speed 2
(spindle base specification parameters #3037 to #3040) Smax : Maximum rotation speed (spindle base specification parameters #3005 to
#3008) T1 : Tap time constant (spindle base specification parameters #3017 to #3020) T2 : Synchronous tap changeover time constant 2
(spindle base specification parameters #3041 to #3044)
13. Program Support Functions 13.1 Fixed Cycles
269
(ii) When synchronous tap changeover spindle rotation speed 2 < spindle rotation speed during return
Smax S2 S(S1)
S1 S2
S'(Smax)
T1
T2 T1T1
T1
T2
T3
T3
S : Command spindle rotation speed S’ : Spindle rotation speed during return S1 : Tap rotation speed (spindle base specification parameters #3013 to #3016) S2 : Synchronous tap changeover spindle rotation speed 2
(spindle base specification parameters #3037 to #3040) Smax : Maximum rotation speed (spindle base specification parameters #3005 to
#3008) T1 : Tap time constant (spindle base specification parameters #3017 to #3020) T2 : Synchronous tap changeover time constant 2
(spindle base specification parameters #3041 to #3044) T3 : Synchronous tap changeover time constant 3
(spindle base specification parameters #3045 to #3048)
13. Program Support Functions 13.1 Fixed Cycles
270
(l) G75 (Fine boring)
Circle cutting cycle performs a series of the cutting as follows: First: positioning of X and Y axes to the circle center. Next: cutting in with Z axis to the commanded position. Then: moving the perfect round cutting the inside of the circle. Until: returning to the circle center. Program G75 Xx1 Yy1 Zz1 Rr1 Qq1 Pp1 Ff1 ; The operation stops at after the (1), (2) and (6) commands during single block operation.
(4)
G98 d
G99 mode
(1)
(2)
(3)
(6)
(7)
x1 , y1
z1
r1
(5)
(7)
r
q1
Y
X
Z
X
(1) G0 Xx1 Yy1
(2) G0 Zr1
(3) G1 Zz1 Ff1
(4) Gn X-(q1-r) I-(q1/2)
Inner circumference half circle
(5) Iq1 Outer circumference
(6) X(q1-r) I(q1/2)
Inner circumference half circle (7) G98 mode G0 Z-(z1+r1) G99 mode G0 Z-z1 n:q1 0 : G02
q1 < 0 : G03
r: Tool radius compensation amount of the No.
commanded with p1″
13. Program Support Functions 13.1 Fixed Cycles
271
(m) G76 (Fine boring)
Program G76 Xx1 Yy1 Zz1 Rr1 Iq1 Jq2 Ff1 ;
(1) G0 Xx1 Yy1 (2) G0 Zr1 (3) G1 Zz1 Ff1 (4) M19 (Spindle orient) (5) G1 Xq1 (Yq2) Ff1 (Shift) G98 mode G0Z (z1+r1) G99 mode G0Z z1 (7) G0 X q1 (Y q2) Ff1 (Shift) (8) M3 (Spindle forward rotation)
G98 G99 mode mode
(4)(5)
(1)
x1 , y1
z1
r1(2)
(8)
(3)
(6)
(6)
(7)
(7)
(8)
(6)
The operation stops at after the (1), (2) and (7) commands during single block operation. When this command is used, high precision drilling machining that does not scratch the machining surface can be done. (Positioning to the hole bottom and the escape (return) after cutting is executed in the state shifted to the direction opposite of the cutter.)
Spindle orient position
Tool during cutting
Cancel
Tool after cutting
Machining hole
Cutter
Shift
Cancel
Shift
Shift amount
Command I, J, and K with incremental values in the same block as the hole position data. I, J and K will be handled as modals during the canned cycle.
(Note) If the parameter «#1080 Dril_z» which fixes the hole drilling axis to the Z axis is
set, the shift amount can be designated with address Q instead of I and J. In this case, whether to shift or not and the shift direction are set with parameter «#8207 G76/87 IGNR» and «#8208 G76/87 ()». The symbol for the Q value is ignored and the value is handled as a positive value.
The Q value is a modal during the canned cycle, and will also be used as the G83, G87 and G73 cutting amount.
The shift amount is designated as shown below with addresses I, J and K. For G17 : I, J For G18 : K, I For G19 : J, K The shift amount is executed with linear interpolation, and the feed rate follows the F command.
13. Program Support Functions 13.1 Fixed Cycles
272
Precautions for using canned cycle
(1) Before the canned cycle is commanded, the spindle must be rotating in a specific direction
with an M command (M3 ; or M4 ;). Note that for the G87 (back boring) command, the spindle rotation command is included in the canned cycle so only the rotation speed command needs to be commanded beforehand.
(2) If there is a basic axis, additional axis or R data in the block during the canned cycle mode, the hole drilling operation will be executed. If there is not data, the hole will not be drilled. Note that in the X axis data, if the data is a dwell (G04) time command, the hole will not be drilled.
(3) Command the hole machining data (Q, P, I, J, K) in a block where hole drilling is executed. (Block containing a basic axis, additional axis or R data.)
(4) The canned cycle can be canceled by the G00 to G03 or G33 command besides the G80 command. If these are designated in the same block as the canned cycle, the following will occur.
(Where, 00 to 03 and 33 are m, and the canned cycle code is n) Gm Gn X___Y___Z___R___Q___P___L___F___; Execute Ignore Execute Ignore Record Gm Gn X___Y___Z___R___Q___P___L___F___; Ignore Execute Ignore Record
Note that for the G02 and G03 commands, R will be handled as the arc radius. (5) If an M function is commanded in the same block as the canned cycle command, the M code
and MF will be output during the initial positioning. The next operation will be moved to with FIN (finish signal). If there is a No. of times designated, the above control will be executed only on the first time.
(6) If another control axis (ex., rotary axis, additional axis) is commanded in the same block as the canned cycle control axis, the canned cycle will be executed after the other control axis is moved first.
(7) If the No. of repetitions L is not designated, L1 will be set. If L0 is designated in the same block as the canned cycle G code command, the hole machining data will be recorded, but the hole machining will not be executed. (Example) G73X___Y___Z___R___Q___P___F___L0___;
Execute Record only code having an address (8) When the canned cycle is executed, only the modal command commanded in the canned
cycle program will be valid in the canned cycle subprogram. The modal of the program that called out the canned cycle will not be affected.
(9) Other subprograms cannot be called from the canned cycle subprogram. (10) Decimal points in the movement command will be ignored during the canned cycle
subprogram. (11) If the No. of repetitions L is 2 or more during the incremental value mode, the positioning will
also be incremented each time. (Example) G91G81X10. Z50.R20.F100.L3 ;
X
Z 10. 10. 10.
13. Program Support Functions 13.1 Fixed Cycles
273
(12) If the spindle rotation speed value during return is smaller than the spindle speed, the spindle
rotation speed value is valid even during return. (13) If the 2nd and 3rd acceleration/deceleration stage inclinations following the spindle rotation
speed and time constants set in the parameters are each steeper than the previous stage’s inclination, the previous stage’s inclination will be valid.
(14) If the values set in the spindle base specification parameter «stap1-4» (tap rotation speed) and «taps21-24» (synchronous tap changeover spindle rotation speed 2) exceed the maximum rotation speed, the spindle rotation speed will be clamped at the maximum rotation speed.
(15) If the spindle rotation speed during return is not 0, the tap return override value will be invalid. (16) In a block where the movement direction of any axis reverses as shown below, the servo
system load will greatly increase so do not command the in-position width in the machining program.
G0 X100., I10.0 ; X-200. ; (17) If the in-position width commanded with the programmable in-position width command is
increased, the positioning time and linear interpolation time can be reduced. However, the position error amount of the previous block will also increase before the next block starts, so the actual machining could be obstructed.
(18) The in-position width and the position error amount are compared at a set time, so the position error amount at the point to be judged as in-position will be smaller than the commanded in-position width.
(19) If the in-position width commanded with the programmable in-position command is small, the commanded deceleration check or in-position check following the parameters may be carried out first.
(20) Synchronous and asynchronous tap can be selected with the M function. Base specifications parameters
# Items Details Setting range
1272 (PR) ext08 bit1 M-function synchronous tap cycle valid. 0:Invalid
1:Valid Synchronous tap cannot be selected with the M function when this parameter is OFF. Base specifications parameters
# Items Details Setting range
1513 stapM M code for synchronous tap selection 0 to 99999999 The synchronous tap mode is selected with the miscellaneous function code set with this parameter. The M function can be commanded in the same block before the tap command.
The synchronous and asynchronous tap will follow the combination shown below. Combination Program command (,R0/1) 0 0 0 0 1 1 1 1 No command #1229 (bit4) (Synchronous tap valid) 0 0 1 1 0 0 1 1 0 0 1 1
M function code (M**) Synchronous/ asynchronous selection A A A A S S S S A S S S
: Does not command A : Asynchronous tap : Commands S : Synchronous tap
(Note1) Do not use M00, 01, 02, 30, 98 or 99. (Note2) Depending on the model, selection with the M function may not be possible.
(21) Even when the parameter #1151 rstinit is OFF, the fixed cycle will be canceled if NC reset 1
is carried out while executing the fixed cycle.
13. Program Support Functions 13.1 Fixed Cycles
274
13.1.2 Drilling Cycle with High-Speed Retract
Function And Purpose
This function retracts the drill from the hole bottom at high speed in drilling machining. This function helps extending the drill life by reducing the time of drilling in vain at hole bottom.
Hole bottom Moves up at high-speed
Returns in rapid traverse
The drill moves up at high-speed and returns to initial point or R point in rapid traverse
Command Format
Same as the fixed cycle command format.
Detailed Description
(1) This function is available only when #8123 H-spd retract ON is enabled in the following fixed
cycles. G81 (Drill spot drilling cycle) G83 (Deep whole drilling cycle) G73 (Step cycle)
(2) When #8123 H-spd retract ON is ON, the axis is retracted from the hole bottom at high speed
with lost motion compensation. (a) Set the lost motion compensation type 2 or 3 with servo parameter. Then set the following
parameters to adjust the retract amount. #2170 Lmc1QR (Lost motion compensation gain 1 for high-speed retract) (equivalent to «#2216 SV016 LMC1 Lost motion compensation 1») #2171 Lmc2QR (Lost motion compensation gain 2 for high-speed retract) (equivalent to «#2241 SV041 LMC2 Lost motion compensation 2»)
(b) Set the following parameters for lost motion compensation timing or lost motion
compensation 3 spring constant/ viscous coefficient in addition to the ordinary lost motion compensations. #2172 LmcdQR (Lost motion compensation timing for high-speed retract) (equivalent to «#2239 SV039 LMCD Lost motion compensation timing») #2173 LmckQR (Lost motion compensation 3 spring constant for high-speed retract) (equivalent to «#2285 SV085 LMCk Lost motion compensation 3 spring constant») #2174 LmccQR (Lost motion compensation 3 viscous coefficient for high-speed retract) (equivalent to «#2286 SV086 LMCc Lost motion compensation 3 viscous coefficient»)
13. Program Support Functions 13.1 Fixed Cycles
275
(c) If the drilling axis is synchronously controlled, set the same value in both parameters for
primary and secondary axes.
(3) While G80 (Fixed cycle cancel) command is issued, this function is canceled by issuing any other fixed cycle of the same group (Group 9) or any Group 1 command.
(4) This function is invalid during the following command modal.
In this case, the drill moves in the ordinary rapid traverse even if «#8123 H-spd retract ON» is enabled. G43.1 (Tool length compensation in the tool axis direction) G43.4, G43.5 (Tool center point control) G68 (3-dimensional coordinate conversion)
Detailed Description
(1) Operation at G81 command
Start point Initial point G98 mode
R point G99 mode
Retracted at high-speed
(1) (2)
(3)
(4)
(5)
(1) Moves from start point to initial point (2) Moves from initial point to R point (3) Cutting feed (4) Retracted at high-speed
During single block operation, the axis stops after (1), (2) and (5) only.
(2) Operation at G83 command
Initial point G98 mode
G99 mode R point
Retracted at high-speed
G83 Return amount
Retracted at high-speed
Retracted at high-speed
(1) Moves from startong point to initial point
(2) Moves from initial point to R point
(3) Cutting feed
(4) Retracted at high-speed
(5) Returns to R point
(6) Moves to the previous cutting feed position
+ G83 return amount position
(7) Cutting feed
(8) Repeat of (4),(5),(6),and(7)
(9) Retracted at high-speed
(10) Returns to R point or initail point
(1) (2)
(3)
(4)
(5) (6)
(7)
(8)
(9)
(10)
During single block operation, the axis stops after (1), (2) and (10) only.
13. Program Support Functions 13.1 Fixed Cycles
276
(3) Operation of G73 command
Start point Initial point
R point
G98 mode
G99 mode
Retracted
Retracted
at high-speed
at high-speed
G73 Return amount
(1)
(2)
(3)
(4)
(5)
(6)
(7)
(8)
(1) Moves from start point to initial point
(2) Moves from initial point to R point
(3) Cutting feed
(4) Retracted at high-speed
(5) Moves to the position set
with G73 return amount
(6) Repeat of (3),(4), and (5)
(7) Retracted at high-speed
(8) Returns to R point or initial point
During single block operation, the axis stops after (1), (2) and (8) only.
If a dwell command is issued, the high-speed retract will be executed after the command.
13. Program Support Functions 13.1 Fixed Cycles
277
13.1.3 Initial Point and R Point Level Return; G98, G99
Function and purpose
Whether to use R point or initial level for the return level in the final sequence of the canned cycle can be selected.
Command format
G98 ; G99 ; G98 ; Initial level return G99 ; R point level return
Detailed description
The relation of the G98/G99 mode and No. of repetition designation is as shown below.
No. of hole drilling
Program example
G98 At power ON, at cancel with M02, M30, and reset
button G99
Only one execution
G81X100. Y100. Z50. R25. F1000;
Initial point
R point
Initial level return is executed.
Initial point
R point
R point level return is executed.
Second and following executions
G81X100. Y100. Z50. R25. L5F1000;
Second time
Final time
First time
Initial level return is executed for all times.
Second time
Final time
First time
Example of program
(Example 1)
G82 Zz1 Rr1 Pp1 Ff1 L0 ; Record only the hold machining data (Do not execute)
Xx1 Yy1 ; Execute hole drilling operation with G82 mode The No. of canned cycle repetitions is designated with L. If L1 is designated or L not designated, the canned cycle will be executed once. The setting range is 1 to 9999. If L0 is commanded, only the hole machining data will be recorded. G8 (7) Xx1 Yy1 Zz1 Rr1 Pp1 Qq1 Ff1 Ll1 ;
13. Program Support Functions 13.1 Fixed Cycles
278
The ideology of the data differs between the absolute value mode (G90) and incremental value mode (G91) as shown below.
Z axis absolute value zero point
R point R
Z
R point R
Z
Absolute value mode (G90) Incremental value mode (G91)
Designate a command value with a symbol for X, Y and Z. R indicates the coordinate value from the zero point in the absolute value mode, so a symbol must always be added. However, in the incremental value the symbol will be ignored and will be viewed as the same symbol as for Z. Note that the symbols will be viewed in reverse for G87. The hole machining data is held as shown below in the canned cycle. The hole machining data is canceled when the G80 command or G commands (G00, G01, G02, G03, G2.1, G3.1, G33) in the 01 group are reached.
(Example 2) N001 G81 Xx1 Yy1 Zz1 Rr1 Ff1 ;
N002 G81 ;Only selection of canned cycle sequence N003 Xx2 Yy2 ;Change of positioning point, and execution of canned cycle N004 M22 ;Execution of only M22 N005 G04 Xx3 ;Execution of only dwell N006 G92 Xx4 Yy4 ;Execution of only coordinate system setting N007 G28 (G30) Z0 ;Execution of only reference position (zero point) return N008 ; No work N009 G99 Zz2 Rr2 Ff2 L0 ;Execution of only hole machining data recording N010 Xx5 Yy5 Ll5 ;Change of positioning point, and execution of R point return canned
cycle for I5 times N011 G98 Xx6 Yy6 Zz6 Rr6 ;Change of positioning point, and execution of canned cycle N012 Ww1 ;Execute W axis according to 01 group modal before N001, and then
execute canned cycle 13.1.4 Setting of Workpiece Coordinates in Fixed Cycle Mode
The designated axis moves with the workpiece coordinate system set for the axis. The Z axis is valid after the R point positioning after positioning or from Z axis movement.
(Note) When the workpiece coordinates are changed over for address Z and R, re-program
even if the values are the same. (Example) G54 Xx1 Yy1 Zz1 ; G81 Xx2 Yy2 Zz2 Rr2 ; G55 Xx3 Yy3 Zz2 Rr2 ;Re-command even if Z and R are the same as the previous value. Xx4 Yy4 ; Xx5 Yy5 ;
13. Program Support Functions 13.2 Special Fixed Cycle; G34, G35, G36, G37.1
279
13.2 Special Fixed Cycle; G34, G35, G36, G37.1
Function and purpose
The special fixed cycle is used with the standard fixed cycle. Before using the special fixed cycle, program the fixed cycle sequence selection G code and hole machining data to record the hole machining data. (If there is no positioning data, the fixed cycle will not be executed, and only the data will be recorded.) The axis is positioned to the hole machining position when the special fixed cycle is executed. The hole machining operation is executed with the canned cycle for hole machining. Even after the special fixed cycle is executed, the recorded standard fixed cycled will be held until canceled. If the special fixed cycle is designated when not in the fixed cycle mode, only positioning will be executed, and the hole drilling operation will not be done. If the special fixed cycle is commanded without commanding the fixed cycle for hole machining, positioning will be executed following the current 01 group modal G code.
13. Program Support Functions 13.2 Special Fixed Cycle; G34, G35, G36, G37.1
280
Bolt hole circle (G34)
G34 X x1 Y y1 I r J K n ;
X, Y :Positioning of bolt hole cycle center. This will be affected by G90/G91. I :Radius r of the circle. The unit follows the input setting unit, and is given with a
positive number. J :Angle of the point to be drilled first. The CCW direction is positive.
(The decimal point position will be the degree class. If there is no decimal point, the unit will be 0.001.)
K :No. of holes n to be drilled. 1 to 9999 can be designated, but 0 cannot be designated. When the value is positive, positioning will take place in the CCW direction, and when negative, will take place in the CW direction. If 0 is designated, the program error (P221) will occur.
Drilling of n obtained by dividing the circumference by n will start at point created by the Z axis and angle . The circumference is that of the radius R centering on the coordinates designated with XX and Y. The hole drilling operation at each hole will hold the drilling data for the standard canned cycle such as G81. The movement between hole positions will all be done in the G00 mode. G34 will not hold the data even when the command is completed. (Example)
With 0.001mm least command increment
Position prior to excution of G34 command
G0 command in N005
N001 G91 ; N002 G81 Z 10.000 R5.000 L0 F200 ; N003 G90 G34 X200.000 Y100.000 I100.000 J20.000 K6 ; N004 G80 ; …………………….(G81 cancel) N005 G90 G0 X500.000 Y100.000 ;
(500 mm, 100 mm)
20
n = 6 holes
I = 100 mm
X1 = 200 mm
Y1 = 100 mm
W
(Example)
As shown in the example, the tool position after the G34 command is completed is over the final hole. When moving to the next position, the coordinate value must be calculated to issue the command with an incremental value. Thus, use of the absolute value mode is handy. (Note 1) If an address other than the selected plane’s vertical axis, horizontal axis, G, N,
I, J, K, H, O, P, F, M, S or 2nd miscellaneous function is issued in the same block as the G34 command, a program error (P32) will occur.
13. Program Support Functions 13.2 Special Fixed Cycle; G34, G35, G36, G37.1
281
Line at angle (G35)
G35 X x1 Y y1 I d J K n ;
X, Y :Designation of start point coordinates. This will be affected by G90/G91. I :Interval d. The unit follows the input setting unit. If d is negative, the drilling will
take place in the direction symmetrical to the point that is the center of the start point.
J :Angle . The CCW direction is positive. (The decimal point position will be the degree class. If there is no decimal point, the unit will be 0.001.)
K :No. of holes n to be drilled. 1 to 9999 can be designated, and the start point is included.
Using the position designated by X and Y as the start point, the Zn holes will be drilled with interval d in the direction created by X axis and angle . The hole drilling operation at each hole position will be determined by the standard canned cycle, so the hole drilling data (hole machining mode and hole machining data) must be held beforehand. The movement between hole positions will all be done in the G00 mode. G35 will not hold the data even when the command is completed.
(Example)
n=5 holes
Position before G35 is executed
=30
d=100mm
x1=200mm
When input setting unit is 0.001mm
G91 ; G81 Z 10000 R5000 L0 F100 ; G35 X200000 Y100000 I100000 J30000 K5 ;
y1=100mm
(Note 1) If the K command is K0 or if there is no K command, the program error (P221)
will occur. (Note 2) If the K value is more than four digits, the last four digits will be valid. (Note 3) If an address other than the selected plane’s vertical axis, horizontal axis, G, N,
I, J, K, H, O, P, F, M, S or 2nd miscellaneous function is issued in the same block as the G35 command, a program error (P32) will occur.
(Note 4) If a group 0 G command is issued in the same block as the G35 command, the command issued later is the priority. (Example) G35 G28 Xx1 Yy1 Ii1 Jj1 Kk1 ;
G35 is ignored G 28 is executed as Xx1 Yy1 (Note 5) If there is a G72 to G89 command in the same block as the G35 command, the
canned cycle will be ignored, and the G35 command will be executed.
13. Program Support Functions 13.2 Special Fixed Cycle; G34, G35, G36, G37.1
282
Arc (G36)
G36 X x1 Y y1 I r J P K n ;
X, Y :Center coordinates of arc. This will be affected by G90/G91. I :Radius r of arc. The unit follows the input setting unit, and is given with a positive
No. J :Angle of the point to be drilled first. The CCW direction is positive. (The decimal
point position will be the degree class. If there is no decimal point, the unit will be 0.001.)
P :Angle interval . When the value is positive, the drilling will take place in the CCW direction, and in the CW direction when negative. (The decimal point position will be the degree class. If there is no decimal point, the unit will be 0.001.)
K :No. of holes n to be drilled. 1 to 9999 can be designated.
The n holes aligned at the angle interval will be drilled starting at point created by the X axis and angle . The circumference is that of the radius R centering on the coordinates designated with XX and Y. As with the bolt hole circle, the hole drilling operation at each hole will depend on the standard canned cycle. The movement between hole positions will all be done in the G00 mode. G36 will not hold the data even when the command is completed. (Example)
n=6 holes
x1=300mm
=10
= 15
y1=100mm
Position before G36 is executed
When input setting unit is 0.001mm
N001 G91 ; N002 G81 Z 10000 R5000 F100 ; N003 G36 X300000 Y100000 I300000 J10000 P15000 K6 ;
(Note 1) If an address other than the selected plane’s vertical axis, horizontal axis, G, N,
I, J, K, H, O, P, F, M, S or 2nd miscellaneous function is issued in the same block as the G36 command, a program error (P32) will occur.
13. Program Support Functions 13.2 Special Fixed Cycle; G34, G35, G36, G37.1
283
Grid (G37.1)
G37.1 X x1 Y y1 I Dx P nx J Dy K ny ;
X, Y :Designation of start point coordinates. This will be affected by G90/G91. I :Interval Dx of the X axis. The unit will follow the input setting unit. If Dx is positive,
the interval will be in the forward direction looking from the start point, and when negative, will be in the reverse direction looking from the start point.
P :No. of holes nx in the X axis direction. The setting range is 1 to 9999. J :Interval Dy of the Y axis. The unit will follow the input setting unit. If Dy is positive,
the interval will be in the forward direction looking from the start point, and when negative, will be in the reverse direction looking from the start point.
K :No. of holes ny in the Y axis direction. The setting range is 1 to 9999.
The nx points on a grid are drilled with an interval x parallel to the X axis, starting at the position designated with X, Y. The drilling operation at each hole position will depend on the standard canned cycle, so the hole drilling data (hole machining mode and hole machining data) must be held beforehand. The movement between hole positions will all be done in the G00 mode. G37.1 will not hold the data even when the command is completed.
(Example)
ny=8 holes Position before G37 is executed
nx=10 holes x1=300mm
y= 100mm
y1=100mm
x=50mm
When input setting unit is 0.01mm
G91 ; G81 Z 10000 R5000 F20 ; G37.1 X300000 Y100000 I50000 P10 J100000 K8 ;
(Note 1) If the P and K commands are P0 or K0, or if there is no P or K command, the
program error (P221) will occur. If the P or K value is more than four digits, the last four digits will be valid. (Note 2) If an address other than the selected plane’s vertical axis, horizontal axis, G, N,
I, J, K, H, O, P, F, M, S or 2nd miscellaneous function is issued in the same block as the G37.1 command, a program error (P32) will occur.
(Note 3) If a group 0 G command is issued in the same block as the G37.1 command, the command issued later is the priority.
(Note 4) If there is a G72 to G89 command in the same block as the G37.1 command, the canned cycle will be ignored, and the G37.1 command will be executed.
(Note 5) If the G22/G23 command is programmed in the same block as the G37.1 command, the G22/G23 command will be ignored, and the G37.1 command will be executed.
13. Program Support Functions 13.3 Subprogram Control; M98, M99, M198
284
13.3 Subprogram Control; M98, M99, M198 13.3.1 Calling Subprogram with M98 and M99 Commands
Function and purpose
Fixed sequences or repeatedly used parameters can be stored in the memory as subprograms which can then be called from the main program when required. M98 serves to call subprograms and M99 serves to return operation from the subprogram to the main program. Furthermore, it is possible to call other subprograms from particular subprograms and the nesting depth can include as many as 8 levels.
Main program O0010; M98 P1000; M02;
Subprogram O1000; M98 P1200
H20; M99;
(Level 1)
Subprogram O1200; N20; M98 P2000; N60; M99;
Subprogram O2000; M98 P2500; M99 P60;
Subprogram O3000; M99;
(Level 2) (Level 3) (Level
Nesting depth
The table below shows the functions which can be executed by adding and combining the tape storing and editing functions, subprogram control functions and fixed cycle functions.
Case 1 Case 2 Case 3 Case 4 1. Tape storing and editing Yes Yes Yes Yes 2. Subprogram control No Yes Yes No 3. Fixed cycles No No Yes Yes
Function 1. Memory mode 2. Tape editing (main memory) 3. Subprogram call 4. Subprogram variable designation (Note 2) 5. Subprogram nesting level call (Note 3) 6. Fixed cycles 7. Subprogram editing for fixed cycle
(Note 1) » » denotes a function which can be used and «» a function which cannot be used.
(Note 2) Variables cannot be transferred with the M98 command but variable commands in subprograms can be used provided that the variable command option is available.
(Note 3) A maximum of 8 nesting levels form the nesting depth.
13. Program Support Functions 13.3 Subprogram Control; M98, M99, M198
285
Command format
Subprogram call
M98 P__ H__ L__ ,D; or M98 <File name> H__ L__ ,D__ ; M98 Subprogram call command P Program No. of subprogram to be called (own program if omitted)
P can be omitted only during memory mode and MDI mode. (Max. 8 digits)
File name A file name can be specified instead of a program No. In this case, enclose the file name with brackets <>. (The file name can have up to 32 characters including the extension.) (Example) M98
H Sequence No. in subprogram to be called (head block if omitted) (Max. 5 digits)
L Number of subprogram repetitions (When omitted, this is interpreted at L1, and is not executed when L0.) (Between 1 and 9999 times according to 4-digit value.) For instance, M98 P1 L3 ; is equivalent to the following: M98 P1 ; M98 P1 ; M98 P1 ;
,D Subprogram device No. (0 to 4). The subprogram in the memory can be used when ,D is omitted. The device No. is set with the machining parameters.
Return to main program from subprogram
M99 P__ ; M99 Subprogram return command P Sequence No. of return destination (returned to block that follows the calling
block)
Creating and entering subprograms
Subprograms have the same format as machining programs for normal memory mode except that the subprogram completion instruction M99 (P_ L_ ) ; is entered as an independent block at the last block.
; Program No. as subprogram No. ………………………….. ; ………………………….. ; : Main body of subprogram : : ………………………….. ; M99 ; Subprogram return command % (EOR) Entry completion code
(1) The above program is entered by editing operations at the setting and display unit. For further details, refer to the section on program editing in the Instruction Manual.
13. Program Support Functions 13.3 Subprogram Control; M98, M99, M198
286
(2) Only those subprograms Nos. ranging from 1 to 99999999 designated by the optional specifications can be used. When there are no program Nos. on the tape, they are entered as the setting No. for «program input.»
(3) Up to 8 nesting levels can be used for calling programs from subprograms, and program error (P230) results if this number is exceeded.
(4) No distinction between main programs and subprograms is made since they are entered in the sequence in which they were read. This means that main programs and subprograms should not be given the same Nos. (If they are, error «E11» appears during entry.)
(5) Besides the M98 command, subprogram nesting is subject to the following commands:
G65 : Macro call G66 : Modal call G66.1 : Modal call G code call Miscellaneous function call MDI interruption Automatic tool length measurement Macro interruption Multiple-step skip function
(6) Subprogram nesting is not subject to the following commands which can be called even beyond the 8th nesting level.
Fixed cycles Pattern cycles
(7) To repeatedly use the subprogram, it can be repeated l1 times by programming M98 Pp1 Ll1;.
(8) When using the multi-part system, if the subprogram attributed to the part system with the call command is empty, the subprogram call operation will change according to the parameters.
#1050 MemPrg
#1285 ext21/bit1 Details
0, 2, 4, 6 — The subprogram registered in the memory common for the part systems is called out.
1, 3, 5, 7 OFF The subprogram registered in the memory for the selected part system is called out.
ON The subprogram registered in the memory for the selected part system is called out. If the subprogram in the selected part system is empty, the subprogram with the same No. in the 1st part system is called out.
13. Program Support Functions 13.3 Subprogram Control; M98, M99, M198
287
Example of program 1
When there are 3 subprogram calls (known as 3 nesting levels)
M98P1;
M02;
Main program Subprogram 1 Subprogram 2 Subprogram 3
Sequence of execution : (1) (2) (3) (3) (2) (1)
(1)
O1; M98P10;
M99;
O10; M98P20;
M99;
O20;
M99;
(1)
(2)
(2)
(3)
(3)
(1) For nesting, the M98 and M99 commands should always be paired off on a 1:1 basis (1) for (1), (2)’ for (2), etc.
(2) Modal information can be rewritten according to the execution sequence without distinction between main programs and subprograms. This means that after calling a subprogram, attention must be paid to the modal data status when programming.
13. Program Support Functions 13.3 Subprogram Control; M98, M99, M198
288
Example of program 2
The M98 H_ ; M99 P_ ; commands designate the sequence Nos. in a program with a call instruction.
M98H3;
N3___;
M99;
M98H__ ;
N100___;
M98P123; N200_; N300___; N400___;
O123; M99P200;
M99P__ ;
S ea
rc h
Precautions
(1) Program error (P232) results when the designated P (program No.) is not located.
(2) Single block stop does not occur with the M98 P_ ; M99 ; block. If any address except O, N, P, L or H is used, single block stop can be executed. (With X100. M98 P100 ;, operation branches to O100 after X100. is executed.)
(3) When M99 is commanded by the main program, operation returns to the head. (This is same for MDI.)
(4) Branching from tape and BTR operation to the subprogram with M98 P_ is possible, but the return destination sequence No. cannot be designated with M99 P_ ;. (P_ is ignored).
(5) Bear in mind that the search operation will take time when the sequence No. is designated by M99 P_ ;.
(6) When using a file name for the subprogram, specify the file name with 32 characters or less, including the extension. If a file name exceeding 32 characters is specified, a program error (P232) will occur.
(7) All the programs are registered as files. For example, when calling the file «0100» as a subprogram, «0100» cannot be searched with M98P100 or M98P0100. When a value is specified following P, reading 0 is omitted; therefore, it is assumed that the program No. (file) «100» was specified in this case. When wishing the program like «0100» to be called, specify the file name using the M98<0100> format.
13. Program Support Functions 13.3 Subprogram Control; M98, M99, M198
289
13.3.2 Calling Subprogram with M198 Commands
Function and purpose
Programs saved in the data server can be called as subprograms. To call a program in the data server as a subprogram, command in the main program as shown below.
Command format
Calling Subprogram
M198 P__ L__ ; or M198 <File name> L__ ; M198 Subprogram call command P Program No. in data server to be called as subprogram. (Max. 8 digits) File name
A file name can be specified instead of a program No. In this case, enclose the file name with brackets <>. (The file name can have up to 32 characters including the extension.)
L Number of subprogram repetitions. (Max. 4 digits) This can be omitted. (In this case, the subprogram will be called once.)
When «L0» is designated, the subprogram call will not be executed. (Note) Sequence No. call (M198 H***) cannot be commanded. Return to main program from subprogram
M99 ;
Detailed description
(1) The subprogram can be called with the M198 command once in the subprogram nest. The
subprogram can be called only from the memory or MDI program.
(2) The section from the head of the program to the first LF (carriage return code, 0x0A hexadecimal) is invalid, and is not run or displayed. Note that if the head starts with a 0 No., the program will be valid from the head.
(3) A program registered in an IC card can be executed from only one part system. A program error will occur if it is attempted to execute the programs in the IC card simultaneously by two or more part systems. When the reset is applied on all the part systems, the program of 2nd and following part systems may be displayed as only «%».
(4) Refer to «13.3.1 Calling subprogram with M98 and M99 commands» for .
13.3.3 Figure Rotation; M98 I_ J_ K_
Function and purpose
If the same pattern is used repeatedly on a concentric circle, one of the rotating machining patterns can be registered as a subprogram. When the subprogram is called from the main program, if the rotation center is designated, a path similar to the rotary phase can be easily created on the concentric circle. This simplifies creation of the program.
13. Program Support Functions 13.3 Subprogram Control; M98, M99, M198
290
Command format
M98 I__ J__ K__ P__ H__ L__ ,D__; or, M98 I__ J__ K__ H__ L__ ,D__ ;
M98 I, J, K P
: Subprogram call command : Rotation center : Program No. in subprogram to be called. (Own program if omitted.)
Note that P can be omitted only during memory operation and MDI operation. (Max. 8-digit value)
: A file name can be designated instead of the program No. In this case, enclosed the file name with brackets <>. (The file name can have up to 32 characters, including the extension.) (Example) M98 ;
H
: Sequence No. in subprogram to be called (Head block if omitted) (Max. 5-digit value)
L :
Number of subprogram repetitions (If omitted, this is handled as L1. When L0 is set, the subprogram is not called.) (1 to 9999 times set with 4-digit value.)
,D Subprogram device No. (0 to 4). The subprogram in the memory can be used when ,D is omitted. The device No. is set with the machining parameters.
Detailed description
P1 times Basic figure
j1
i1 Rotation center
(1) The first subprogram called out with subprogram call is executed at a 0 rotation angle. The path is created as commanded.
(2) If the number of repetitions is set to two or more, the rotation angle is obtained from the called subprogram’s start point, end point and rotation center coordinate. The path of the first subprogram is used as a basic figure and is rotated and arranged for the designated number of call repetitions, using the rotation center coordinates as a reference.
(3) All blocks in the subprogram are rotated. (4) If the subprogram start point and end point are not on the same circle having the commanded
figure rotation center coordinates as the center, the axis will interpolate using the subprogram’s end point as the start point, and the end point in the first movement command block in the rotated subprogram as the end point.
13. Program Support Functions 13.3 Subprogram Control; M98, M99, M198
291
(5) Both absolute values and incremental values can be used in the figure rotation subprogram.
Even if commanded with an absolute value command, the rotation will be the same as when commanded with an incremental value.
(6) I, J, and K are commanded with the incremental amount from the start point. (7) A subprogram of which figure is rotating cannot be branched to the other subprogram. (8) The figure is rotated on the workpiece coordinate system, and can be shifted with the G92,
G52, G54 to G59 (workpiece coordinate system shift) command. (9) Functions (reference position return, unidirectional positioning, etc.) on the machine
coordinate system for the rotary plane axis cannot be used while the figure is rotated. However, the machine coordinate system functions can be used for axes other than the rotation plane.
(10) Refer to «13.3.1 Calling subprogram with M98 and M99 commands» for .
Precautions
(1) A program error will occur if figure rotation is commanded during figure rotation. (2) Figure rotation and program coordinate rotation cannot be commanded simultaneously.
Example of program
200.
Main program (L1000) N01 G90 G54 G00 X0 Y0 ; N02 G01 G41 X200. Y150. D01 F500 ; N03 G01 Z-50. F300 ; N04 G22 L2200 P5 J-100. ; N05 G90 G01 Z50. F500 ; N06 G40 ; N07 G00 X0 Y0 ; Subprogram (L2200) N01 G91 G01 X29.389 Y-59.549 ; N02 X65.717 Y-9.549 ; N03 G23 ;
100. 300.
Y
X
Basic figure
13. Program Support Functions 13.4 Variable Commands
292
13.4 Variable Commands
Function and purpose
Programming can be endowed with flexibility and general-purpose capabilities by designating variables, instead of giving direct numerical values to particular addresses in a program, and by assigning the values of those variables as required when executing a program.
Command format
# = or # = [formula]
Detailed description
(1) Variable expressions Example
(a) #m (b) # [f]
m = value consisting of 0 to 9 f = one of the following in the formula
Numerical value m Variable Formula operator formula (minus) formula [Formula] function [formula]
#100 # [-#120] 123 #543 #110+#119 -#120
[#119] SIN [#110]
(Note 1) The 4 standard operators are +, , and /. (Note 2) Functions cannot be used unless the user macro specifications are available. (Note 3) Error «P241» results when a variable number is negative. (Note 4) Examples of incorrect variable expressions are given below.
Incorrect Correct #6/2 #[6/2] (Note that expression such as «#6/2» is regarded as
«[#6] /2») #- -5 #[- [-5]] #- [#1] #[-#1]
13. Program Support Functions 13.4 Variable Commands
293
(2) Type of variables
The following table gives the types of variables. Type of variable No. Function
Common variables Common variables 1
Common variables 2
100 sets 500 to 549 100 to 149 200 sets 500 to 599 100 to 199 300 sets 500 to 699 100 to 199
600 sets
500 to 999 100100 to 800199 (Note 7)
100 to 199
1st part system
700 sets
400 to 999 (Note 4) 100100 to 800199 (Note 7)
100 to 199
50 + 50 * n sets 500 to 549 100 to 149 * n 100 + 100 * n sets 500 to 599 100 to 199 * n 200 + 100 * n sets 500 to 699 100 to 199 * n
500 + 100 * n sets
500 to 999 100100 to 800199 (Note 7)
100 to 199 * n
Multi-part system (n = number of part systems)
600 + 100 * n sets
400 to 999 (Note 4) 100100 to 800199 (Note 7)
100 to 199 * n
Can be used in common throughout main, sub and macro programs.
When using common variables in the multi-part system, the number of common variable shared between the part systems can be specified by the parameter «#1052 MemVal». (Note 5)
Local variables 1 to 33 Can be used for local variables in macro programs.
System variables From 1000 Application is fixed by system.
Fixed cycle variables 1 to 32 Local variables in fixed cycle programs.
(Note 1) All common variables are retained even when the power is turned OFF.
(Note 2) When the power is turned OFF or reset, the common variables can be set to by setting the parameter (#1128 RstVC1, #1129 PwrVC1).
(Note 3) The common variables are divided into the following two types. Common variables 1 : Used in common through all part systems Common variables 2 : Used in common in the programs of the part system
(Note 4) Address #400s common variable can be used only when the sets of common variable is «700 sets» and the parameter «#1336 #400_Valtype» is «1». If address #400s common variable is used when the set of common variable is other than 700 sets or the parameter «#1336 #400_Valtype» is «0», a program error (P241) will occur. When common variable address #400s can be used, these can be displayed and set on the common variable screen. It is possible to input/output data of common variable address #400s.
13. Program Support Functions 13.4 Variable Commands
294
(Note 5) When the parameter «#1052 MemVal» is set to «1» in multi-part system, a part or all of common variable «#100 to #199» and «#500 to #999» can be shared and used between part systems. The number of the shared common variable is set by the parameter «#1303 V1comN» (#100 to set value) and «#1304 V0comN» (#500 to set value). (Example) «10» is set to «#1303 V1comN» «5» is set to «#1304 V0comN» #100 to #109 : Common for the
part systems #500 to #504 : Common for the part systems
#110 to #199 : Each part system #505 to #999 : Each part system When the parameter «#1052 MemVal» is set to «0», the common variables «#100 to #199» are used for each part system, and variables «#500 to #999» are common for the part systems. Address #400s, which can be used as common variable with 700 sets of variable, is common for the part systems regardless of the setting of parameter «#1052 MemVal».
(Note 6) In the common variable data input, when the following illegal variable No. data exist in input file, the illegal variable No. data is ignored and only the correct common variable data is input. Variable data which is not common variables of local variable (#1 to #33) and
system variable (#1000 to ), etc. Variable data to which conditions of number of common variable sets are not
corresponding
(Example) If the #100 to #199, #500 to #599 exist in the input file when the common variable 100 sets (#100 to #149, #500 to #549), the #150 to #199, #550 to #599 are ignored, and #100 to #149, #500 to #549 are input.
(Note 7) When the parameter «#1316 CrossCom» is set to «1», the common variables #100100 to #800199 can be used for common variable shared between the part systems. The common variable shared between part systems which can be used is shown in the table below.
Variable sets Common variables 1 (When «#1316 CrossCom» = «1» 600 sets (500 + 100)
Variable sets specification
700 sets (600 + 100)
#100100 to #100199 (Equivalent to # 100 to #199 in 1st part system) #200100 to #200199 (Equivalent to # 100 to #199 in 2nd part system) #300100 to #300199 (Equivalent to # 100 to #199 in 3rd part system) #400100 to #400199 (Equivalent to # 100 to #199 in 4th part system) #500100 to #500199 #600100 to #600199 #700100 to #700199 #800100 to #800199
When 1-part system
#100100=200
#200105=#100
#300110=#100100
#800199=#500120
Equivalent to #100 = 200 ;
«200» is set to #200105
«200» is set to #300110
The variable value of #500120 is set to #800199
13. Program Support Functions 13.4 Variable Commands
295
When multi-part system «Common variable for each part system #100 to #199» in other part system can be used.
$1
#200100=-100
#101=#200102
#300105=#200103
#110=#500107
«-100» is set to #100 of 2nd part system.
The variable value of #102 of 2nd part system is set to #101
The variable value of #103 of 3rd part system is set to #105
The variable value of #500107 is set to #110
The PLC data reading function cannot be used by using system variable #100100 to #100110, and variable #100100 to #100110 are used as common variable.
The setting of number of common variable shared between the part systems (The parameter #1052 MemVal» is set to «1») is invalid, thus the movement is the same as «0» setting.
When the parameters (#1128 RstVC1, #1129 PwrVC1) are set to «1», the operation is as follows according to expression.
«#1128 RstVC1» (Clear variables by resetting) Common variables shared between the part systems equivalent to #100 to #199 of reset part system are cleared. (Example)When resetting in 1st part system, #100100 to #100199 are cleared.
When resetting in 2nd part system, #200100 to #200199 are cleared.
«#1129 PwrVC1» (Clear variables by power-ON) Common variables shared between the part systems equivalent to #100 to #199 of valid part system are cleared. (Example) In 1st part system, #100100 to #100199 are cleared.
In 2nd part system, #100100 to #100199 and #200100 to #200199 are cleared.
Common variables shared between the part systems #100100 to #800199 can be displayed and set on the common variable screen.
If common variable #100100 to #800199 are used when the set of common variable is other than 600/700 sets or the parameter «#1316 CrossCom» is «0», a program error (P241) will occur.
(3) Variable quotations
Variables can be used for all addresses accept O, N and / (slash).
(a) When the variable value is used directly: X#1…………………………… Value of #1 is used as the X value.
(b) When the complement of the variable value is used: X#2…………………………. Value with the #2 sign changed is used as the X value.
(c) When defining variables: #3 = #5 ……………………… Variable #3 uses the equivalent value of variable #5. #1 = 1000 ………………….. Variable #1 uses the equivalent value 1000 (which is treated as
1000.).
(d) When defining the variable arithmetic formula: #1 = #3 + #2 100……… The value of the operation result of #3 + #2 100. is used as the
#1 value. X [#1 + #3 + 1000] ……… The value of the operation result of #1 + #3 + 1000 is used as the
X value.
13. Program Support Functions 13.4 Variable Commands
296
(Note 1) A variable cannot be defined in the same block as an address. It must be defined in a
separate block. Incorrect Correct
X#1 = #3 + 100; #1 = #3 + 100; X#1;
(Note 2) Up to five sets of square parentheses [ ] may be used. #543 = [[[[[#120]/2+15.]3 #100]/#520 + #125 + #128] #130 + #132] (Note 3) There are no restrictions on the number of characters and number of variables for
variable definition. (Note 4) The variable values should be within a range form 0 to 99999999.
If this range is exceeded, the arithmetic operations may not be conducted properly. (Note 5) The variable definitions are valid from the moment that the variables are actually
defined. #1 = 100 ;………………………… #1 = 100 (Valid from the next command) #1 = 200 #2 = #1 + 200 ; ….. #1 = 200, #2 = 400 (Valid from the next command) #3 = #1 + 300 ;…………………. #3 = 500 (Valid from the next command)
(Note 6) Variable quotations are always regarded as having a decimal point at the end. When #100 = 10, then X#100 ; is treated as X10.
13. Program Support Functions 13.5 User Macro Specifications
297
13.5 User Macro Specifications 13.5.1 User Macro Commands; G65, G66, G66.1, G67
Function and purpose
By combining the user macros with variable commands, it is possible to use macro program call, arithmetic operation, data input/output with PLC, control, decision, branch and many other instructions for measurement and other such applications.
Macro call instruction
O Main program O Macro program
……. ; ……. ;
M30 ; M99 ;
Macro programs use variables, arithmetic instructions and control instructions to create subprograms which function to provide special-purpose control. These special-purpose control functions (macro programs) are called by the macro call instructions exactly when required from the main program. The following G codes are available for the macro call commands.
G code Function G65 User macro Simple call G66 User macro Modal call A (Movement command call) G66.1 User macro Modal call B (Per-block call) G67 User macro Modal call cancel
Detailed description
(1) When the G66 (or 66.1) command is entered, the specified user macro subprogram will be
called after each block has been executed (or after the movement command in the block) with the movement commands has been executed until the G67 (cancel) command is entered.
(2) The G66 (or G66.1) and G67 commands must be paired in the same program.
13. Program Support Functions 13.5 User Macro Specifications
298
13.5.2 Macro Call Command
Function and purpose
Included among the macro call commands are the simple calls which apply only to the instructed block and also modal calls (types A and B) which apply to each block in the call modal.
Simple macro calls
To subprogram
To main program
Main program
G65Pp1Ll1 ;
Subprogram (Oo1)
Oo1 M99
M99 is used to conclude the user macro subprogram.
Format
G65 P__ L__ argument ; or G65 <File name> L__ argument ; G65 Call instruction P Program No. File name
A file name can be specified instead of a program No. In this case, enclose the file name with brackets <>. (The file name can have up to 32 characters including the extension.)
L Number of repetitions Argument Specify variable data
When the argument must be transferred as a local variable to a user macro subprogram, the actual value should be designated after the address. Regardless of the address, a sign and decimal point can be used in the argument. There are 2 ways in which arguments are designated. (1) Argument designation I Format : A_ B_ C_ … X_ Y_ Z_
Detailed description (a) Arguments can be designated using any address except G, L, N, O and P.
(b) Except for I, J and K, there is no need for designation in alphabetical order.
(c) I, J and K must be designated in alphabetical order.
I_ J_ K_ …… Correct J_ I_ K_ …… Incorrect
(d) Addresses which do not need to be designated can be omitted.
(e) The following table shows the correspondence between the addresses which can be designated by argument designation I and the variable Nos. in the user macro main body.
13. Program Support Functions 13.5 User Macro Specifications
299
Address and variable number
correspondence Call instructions and usable address
Argument designation I
address Variable in macro G65, G66 G66.1
A #1 B #2 C #3 D #7 E #8 F #9 G #10 H #11 I #4 J #5 K #6 L #12 M #13 N #14 O #15 P #16 Q #17 R #18 S #19 T #20 U #21 V #22 W #23 X #24 Y #25 Z #26
: Can be used. : Cannot be used.
: Can be used while G66.1 command is modal.
13. Program Support Functions 13.5 User Macro Specifications
300
(2) Argument designation II Format : A__ B__ C__ I__ J__ K__ I__ J__ K__
Detailed description
(a) In addition to address A, B and C, up to 10 groups of arguments with I, J, K serving as 1 group can be designated.
(b) When the same address is duplicated, designate the addresses in the specified order. (c) Addresses which do not need to be designated can be omitted. (d) The following table shows the correspondence between the addresses which can be
designated by argument designation II and the variable numbers in the user macro main body.
Argument
designation II address
Variable within macro
Argument designation II
address
Variable within macro
A # 1 J5 #17 B # 2 K5 #18 C # 3 I6 #19 I1 # 4 J6 #20 J1 # 5 K6 #21 K1 # 6 I7 #22 I2 # 7 J7 #23 J2 # 8 K7 #24 K2 # 9 I8 #25 I3 #10 J8 #26 J3 #11 K8 #27 K3 #12 I9 #28 I4 #13 J9 #29 J4 #14 K9 #30 K4 #15 I10 #31 I5 #16 J10 #32
K10 #33 (Note 1) The numbers 1 through 10 accompanying I, J and K denote the sequence of the
commanded groups and they are not required for the actual instructions.
(3) Using arguments designations I and II together If addresses corresponding to the same variable are commanded when both types I and II are used
to designate arguments, the latter address is valid.
(Example 1)
Call instruction G65 A1.1 B-2.2 D3.3 I4.4 I7.7 ;
Variable
#1 : 1.1 #2 : 2.2 #4 : 4.4 #5 : #6 : #7 : 3.3 7.7
In the above example, the last I7.7 argument is valid when both arguments D3.3 and I7.7 are
commanded for the #7 variable.
13. Program Support Functions 13.5 User Macro Specifications
301
Modal call A (movement command call)
G65Pp1Ll1 ; G67
To subprogram
To main program
Main program Subprogram
Oo1 M99
To subprogram
When the block with a movement command is commanded between G66 and G67, the movement command is first executed and then the designated user macro subprogram is executed. The number of times the subprogram is executed is l1 times with each call. The argument is the same as for a simple call.
Format
G66 P__ L__ argument ; or G66 <File name> L__ argument ; G66 Call instruction P Program No. File name
A file name can be specified instead of a program No. In this case, enclose the file name with brackets <>. (The file name can have up to 32 characters including the extension.)
L Number of repetitions Argument Specify variable data
Detailed description (1) When the G66 command is entered, the specified user macro subprogram will be called after
the movement command in the block with the movement commands has been executed until the G67 (cancel) command is entered.
(2) The G66 and G67 commands must be paired in the same program. A program error will result when G67 is issued without the G66 command.
13. Program Support Functions 13.5 User Macro Specifications
302
(Example) Drill cycle
N1 G90 G54 G0 X0Y0Z0;
N2 G91 G00 X-50.Y-50.Z-200.;
N3 G66 P9010 R-10.Z-30.F100;
N4 X-50.Y-50.;
N5 X-50.;
N6 G67;
To subprogram after axis command execution
To main program
S ub
pr og
ra m
X
O 9010 N10 G00 Z #18 M0; N20 G09 G01 Z #26 F#9; N30 G00 Z- [#18+#26]; M99; ~
S ub
pr og
ra m
W
Y
-150. -100. -50. N1
-100.
-50.
N2 N3
N4 N5
N10
N20 N30
Argument F
To subprogram after axis command execution
Argument R
Argument Z
(Note 1) After the axis command is executed in the main program, the subprogram is executed.
(Note 2) The subprogram is not executed in the blocks following G67.
13. Program Support Functions 13.5 User Macro Specifications
303
Modal call B (for each block)
The specified user macro subprogram is called unconditionally for each command block which is assigned between G66.1 and G67 and the subprogram is executed the specified number of times. Format
G66.1 P__ L__ argument ; or G66.1 <File name> L__ argument ; G66.1 Call instruction P Program No. File name
A file name can be specified instead of a program No. In this case, enclose the file name with brackets <>. (The file name can have up to 32 characters including the extension.)
L Number of repetitions Argument Specify variable data
Detailed description (1) In the G66.1 mode, everything except the O, N and G codes in the various command blocks
which are read are handled as the argument without being executed. Any G code designated last or any N code commanded after anything except O and N will function as the argument.
(2) The same applies as when G65P__ is assigned at the head of a block for all significant blocks in the G66.1 mode.
(Example 1)
N100 G01 G90 X100. Y200. F400 R1000; in the G66.1 L1000; mode is the same as: N100 G65 L1000 G01 G90 X100. Y200. F400 R1000;
(Note 1) The Call is performed even in the G66.1 command block in the G66.1 mode and the correspondence between the argument address and the variable number is the same as for G65 (simple call).
(3) The range of the G and N command values which can be used anew as variables in the G66.1
mode is subject to the restrictions applying to values as normal NC command values. (4) Program number L(O), sequence numbers N and modal G codes are updated as modal
information.
13. Program Support Functions 13.5 User Macro Specifications
304
G code macro call
User macro subprogram with prescribed program numbers can be called merely by issuing the G code command. Format G** argument ;
G** :G code for macro call
Detailed description (1) The above instruction functions in the same way as the instructions below, and parameters are
set for each G code to determine the correspondence with the instructions. a. M98P ; b. G65P argument ; c. G66P argument ; d. G66.1P argument ; When the parameters corresponding to c and d above are set, issue the cancel command
(G67) either in the user macro or after the call code has been commanded so as to cancel the modal call.
(2) The correspondence between the «**» which conducts the macro call and the macro program
number P to be called is set by parameter.
(3) Up to 10 G codes from G100 to G255 can be used with this instruction. (G codes used in the system can also be used with parameter «#1081 Gmac_P»). (Note 1) G101 to G110 and G200 to G202 are user macro I codes, but if the parameters
are set as the G code call codes, the G code call will be the priority, and these codes cannot be used for user macro I.
(4) These commands cannot be issued during a user macro subprogram which has been called
by a G code.
Program example
G16X100. Y100. Z100. F500 ;
O9016 M99 ;
13. Program Support Functions 13.5 User Macro Specifications
305
Miscellaneous command macro call (for M, S, T, B code macro call)
The user macro subprogram of the specified program number can be called merely by issuing an M (or S, T, B) code. (Only entered codes apply for M but all S, T and B codes apply.) Format M** ; (or S** ;, T** ;, B**
M** M code for macro call (or S, T, B code) Detailed description (1) The above instruction functions in the same way as the instructions below, and parameters are
set for each M code to determine the correspondence with the instructions. (Same for S, T and B codes)
a : M98 P ; b : G65 P M** ; c : G66 P M** ; d : G66. 1P M** ;
M98, M** are not output
When the parameters corresponding to c and d above are set, issue the cancel command
(G67) either in the user macro or after the call code has been commanded so as to cancel the modal call.
(2) The correspondence between the «M**» which conducts the macro call and the macro program number P to be called is set by parameter. Up to 10 M codes from M00 to M95 can be entered. Note that the codes to be registered are the codes basically required for the machine, and codes excluding M0, M1, M2, M30 and M96 to M99.
(3) As with M98, it is displayed on the screen display of the setting and display unit but the M codes and MF are not output.
(4) Even if the miscellaneous command entered above is issued during a user macro subprogram
called by the M code, macro call will not result and it will be handled as an ordinary miscellaneous command.
(5) All S, T and B codes call the subprograms in the prescribed program numbers of the
corresponding S, T and B functions. (6) A maximum of 10 M codes can be set. However when not setting all 10. Set the parameters as
shown below.
Setting to call O8000 with type 0 (M98 type) during M20 command Setting to call O8001 with type 0 (M98 type) during M21 command Set parameters not being used as shown on left.
[ MACRO ]
M [01] 20 0 8000 M [02] 21 0 8001 M [03] 9999 0 199999999 M [04] 9999 0 199999999 M [05] 9999 0 199999999 : : : : : : M [10] 9999 0 199999999
13. Program Support Functions 13.5 User Macro Specifications
306
Differences between M98 and G65 commands
(1) The argument can be designated for G65 but not for M98. (2) The sequence number can be designated for M98 but no for G65, G66 and G66.1. (3) M98 executes a subprogram after all the commands except M, P, H and L in the M98 block
have been executed, but G65 branches to the subprogram without any further operation. (4) When any address except O, N, P, H or L is included in the M98 block, single block stop results.
This is not the case with G65. (5) The level of the M98 local variables is fixed but it can be varied in accordance with the nesting
depth for G65. (#1, for instance, has the same significance either before or after M98 but a different significance in each case with G65.)
(6) The M98 nesting depth extends up to 8 levels in combination with G65, G66 and G66.1. The G65 nesting depth extends up to only 4 levels in combination with G66 and G66.1.
Macro call command nesting depth
Up to 4 nesting levels are available for macro subprogram calls based on simple call or modal call. The argument with a macro call instruction is valid only on the called macro level. Since the nesting depth for macro calls extends up to 4 levels, the argument can be used as a local variable for the program with each respective macro call. (Note 1) When a G65, G66, G66.1 G code macro call or miscellaneous command macro call
is conducted, this is regarded as nesting level 1 and the level of the local variables is also incremented by one.
(Note 2) The designated user macro subprogram is called every time the movement command is executed with modal call A. However, when the G66 command has been duplicated, the next user macro subprogram is called every time an axis is moved even with movement commands in the macro.
User macro subprograms are called in sequence from the subprogram commanded last.
(Example 1)
Main program
(p1 call) Macro p1 User macro operation
After Z1 execution
(p2 call)
Macro p1
(p1 cancel)
(p2 cancel) After Z2 execution
After Z3 execution
Macro p1 Macro p1 Macro p1
Macro p2
G66Pp1; Zz1 ; x1 y1 x2 M99
x1 y1 x2
x1 y1 x2
G66Pp2; Zz2 ;
G67 ;
Zz3 ;
G67 ;
Zz4 ; Zz5 ;
M99
M99
13. Program Support Functions 13.5 User Macro Specifications
307
13.5.3 ASCII Code Macro
Function and purpose
A macro program can be called out by setting the correspondence of a subprogram (macro program) pre-registered with the parameters to codes, and then commanding the ASCII code in the machining program. This function can be used in addition to the G, M, S, T and B miscellaneous command macro call function. (Execution example 1) M98 type
Main program Subprogram
O0002 ; : D2000 ; : M30 ;
O200 : : : M99 ;
After outputting 2000 to common variable #146, the program No. 200 subprogram is called with the M98 subprogram call type.
#7401 (ASCII [01] Valid/Invalid) 1 (Valid) #7402 (ASCII [01] Code) D #7403 (ASCII [01] Type) 0 (M98 type) #7404 (ASCII [01] Program No.) 200 #7405 (ASCII [01] Variable) 146
Parameter
(Execution example 2) G65 type
Main program Subprogram
O0003 ; : A500 ; : M30 ;
O3000 : : : M99 ;
After outputting 500 to local variable #1, the program No. 3000 subprogram is called out with the G65 macro call type.
#7411 (ASCII [02] Valid/Invalid) 1 (Valid) #7412 (ASCII [02] Code) A #7413 (ASCII [02] Type) 0 (G65 type) #7414 (ASCII [02] Program No.) 3000 #7415 (ASCII [02] Variable) 100 (Not used)
Parameter
13. Program Support Functions 13.5 User Macro Specifications
308
Command format
; Designates the address and code
: :
ASCII code for calling out macro (one character) Value or expression output to variable (Setting range: 999999.9999)
Detailed description
(1) The command above functions in the same way as that below. The correspondence of
commands is set for each ASCII code with the parameters. 0: M98 P ; 1: G65 P ; 2: G66 P ; 3: G66.1 P ; In order to cancel the modal call while parameters are set for 2 and 3 above, issue the cancel
command (G67) after commanding the call code or the during the user macro.
(2) The ASCII code for calling the macro and the program No. P to be called are set with the parameters.
Up to two ASCII codes can be registered.
(3) The code section is output to the variables, but the output destination differs according to the call type and address.
(a) For M98 type The code section is output to the common variable, and the variable No. is set with the
parameters. When corresponding to the first address (parameter #7401), the section is output to the
common variable where the first variable No. (parameter #7404) is indicating.
(b) For G65/G66/G66.1 type The code section is output to the local variable. The variable No. differs according to the
address, and corresponds to the following table.
Address # Address # Address # A 1 K 6 U 21 B 2 L 12 V 22 C 3 M 13 W 23 D 7 N 14 X 24 E 8 O 15 Y 25 F 9 P 16 Z 26 G 10 Q 17 H 11 R 18 I 4 S 19 J 5 T 20
(Note) The following addresses can be used.
A, B, D, F, H, I, J, K, M, Q, R, S, T
13. Program Support Functions 13.5 User Macro Specifications
309
Restrictions
(1) Calling a macro with an ASCII code from a program macro-called with an ASCII code A macro cannot be called with an ASCII code from a program macro-called with an ASCII
code. The other patterns are shown below. If it is determined that the macro cannot be called, the command will be handled as a normal
command.
Called side ASCII GMSTB
macro G65/66/66.1 M98
ASCII GMSTB macro G65/66/66.1
Calling side
M98
(2) Nest level of macro call command
The macro subprogram can be called in up to four levels using simple call (G65) and modal call (G66/G66.1).
The macro call command’s argument is valid only in the called macro level. Since the macro call nest level is four levels, the argument for each macro call can be used in
the program as a local variable.
(3) Nest level of subprogram call
Counting the main program as 0, up to eight levels of subprograms can be called (G22) from a subprogram.
The following commands are used for subprogram nesting.
(a) G22
(b) G65 G66 G66.1
(c) G code call Miscellaneous function call (M/S/T/B)
(d) MDI interruption
(e) Automatic tool length measurement
(f) Multiple-step skip function The following commands can be commanded regardless of nesting.
(g) Fixed cycle
(h) Macro interruption
13. Program Support Functions 13.5 User Macro Specifications
310
(4) Order of command priority
If «M» is designated for the ASCII code address, the codes basically necessary for that
machine will be overlapped. In this case, commands will be identified with the following priority using code values.
(a) M00 (program stop command), M01 (optional stop command) M02, M30 (end command)
(b) When corresponding to miscellaneous code (M) call macro command
(c) When corresponding to ASCII code macro command
(d) Used as normal command If «S», «T» and «B» are designated for the ASCII code address, commands will be identified with
the following priority using code values.
(a) When corresponding to miscellaneous code (S, T, B) call macro command
(b) When corresponding to ASCII code macro command
(c) Used as normal command If the other addresses do not correspond to the ASCII code macro command, they will be
identified as normal commands. If the command to be used overlaps with an ASCII code macro command, it must be commanded in the program macro-called with the ASCII code.
Note that there are cases where the command will be unconditionally handled as a normal command, as explained in (5) below.
(5) Conditions where the address set in ASCII code macro command is handled as a normal
command
(a) When there is a data setting command (G10) in the same block.
(b) When ASCII code macro call is executed after the G code macro call command in the same block (also applies for M, S, T, B and ASCII)
(Example) When address «D» (G65 type) is set in the ASCII code macro, and M50 is set in the macro call (G65 type).
M50 D200 ; Execute M code macro with argument (Set 200 in #7)
(c) When inputting parameters
(d) When there is a comma (,) before the address. (Example) «,D», «,R», etc.
(e) When commanded in fixed cycle
(f) When commanded in macro subprogram called with G code macro call (Also applies when macro is called with M, S, T, B or ASCII)
13. Program Support Functions 13.5 User Macro Specifications
311
13.5.4 Variables
Function and purpose
Both the variable specifications and user macro specifications are required for the variables which are used with the user macros. The offset amounts of the local, common and system variables among the variables for this MELDAS NC system except #33 are retained even when the unit’s power is switched off. (Common variables can also be cleared by parameter «#1129 PwrVC1».)
Variable multiplexing
When the user macro specifications applied, variable numbers can be turned into variables (multiple use of variables) or replaced by . Only one of the four basic arithmetic rule (+, -, , ) operations can be conducted with .
(Example 1) Multiple use of variables #1 = 10 #10 = 20 #20 = 30 ; #[#[#1]] = #[#10] from #1 = 10. #5 = #[#[#1]] ; #[#10] = #20 from #10 = 20. Therefore, #5 = #20 or #5 = 30.
#1 = 20 #10 = 20 #20 = 30 #5 = 1000 ; #[#[#1]] = #[#10] from #1 = 10. #[#[#1]] = #5 ; #[#10] = #20 from #10 = 20. Therefore, #20 = #5 or #20 = 1000.
(Example 2) Example of multiple designation of variables
#10 = 5 In which case ##10 = 100 ; #5 = 100
##10 = 100; is handled in the same manner as # [#10] = 100.
(Example 3) Replacing variable numbers with
#10 = 5 ; #[#10 + 1] = 1000 ; In which case, #6 = 1000. #[#10 — 1] = -1000 ; In which case, #4 = -1000. #[#103] = 100 ; In which case, #15 = 100. #[#10/2] = -100 ; In which case, #3 = -100. (Rounded off.)
13. Program Support Functions 13.5 User Macro Specifications
312
Undefined variables
Variables applying with the user macro specifications such as variables which have not been used even once after the power was switched on or local variables not quoted by the G65, G66 or G66.1 commands can be used as . Also, variables can forcibly be set to . Variable #0 is always used as the variable and cannot be defined in the left-side member.
(1) Arithmetic expressions #1 = #0 ; ……………….#1 = #2 = #0 + 1 ; …………. #2 = 1 #3 = 1 + #0 ; …………. #3 = 1 #4 = #010 ; …………. #4 = 0 #5 = #0 + #0 ; ……….. #5 = 0
It should be borne in mind that in an arithmetic expression is handled in the same way as 0.
+ = 0 + = Constant + = Constant
(2) Variable quotations When undefined variables only are quoted, they are ignored up to the address. When #1 = G0 X#1 Y1000 ;…………….Equivalent to G0 Y1000 ; G0 X#1 + 10 Y1000 ; …….Equivalent to G0 X10 Y1000 ;
(3) Conditional expressions and 0 are not equivalent for EQ and NE only. (#0 means .)
When #101 = When #101 = 0 #101 EQ #0
= established #101 EQ #0
0 = not established #101 NE 0
0 established #101 NE 0
0 0 not established #101 GE #0
established #101 GE #0
0 established #101 GT 0
> 0 not established #101 GT 0
0 > 0 not established #101 LE #0
established #101 LE #0
0 established #101 LT 0
< 0 not established #101 LT 0
0 < 0 not established (Note 1) EQ and NE should be used only for integers. For comparison of numeric values with
decimals, GE, GT, LE, and LT should be used.
13. Program Support Functions 13.5 User Macro Specifications
313
13.5.5 Types of Variables
Common variables
Common variables can be used commonly from any position. Number of the common variables sets depends on the specifications. Refer to «13.4 Variable commands» for details.
Local variables (#1 to #33)
These can be defined as an when a macro subprogram is called or used locally within main programs and subprograms. They can be duplicated regardless of the relationship existing between macros (up to 4 levels). G65 P__ L__ ; P : Program number
l : Number of repetitions The is assumed to be Aa1 Bb1 Cc1 ………….. Zz1.
The following table shows the correspondences between the addresses designated by and the local variable numbers used in the user macro main bodies.
[Argument specification I] Call command Call command
G65 G66 G66.1
Argument address
Local variable number
G65 G66 G66.1
Argument address
Local variable number
A #1 Q #17 B #2 R #18 C #3 S #19 D #7 T #20 E #8 U #21 F #9 V #22
G #10 W #23
H #11 X #24 I #4 Y #25 J #5 Z #26 K #6 — #27
L #12 — #28
M #13 — #29
N #14 — #30
O #15 — #31
P #16 — #32 — #33
» » in the above table denotes an argument address which cannot be used. However, provided that the G66.1 mode has been established, an argument address denoted by the asterisk can be added for use. «» denotes that a corresponding address is not available.
13. Program Support Functions 13.5 User Macro Specifications
314
[Argument specification II]
Argument specification II address
Variable in macro
Argument specification II address
Variable in macro
A # 1 I6 #19 B # 2 J6 #20 C # 3 K6 #21 I1 # 4 I7 #22 J1 # 5 J7 #23 K1 # 6 K7 #24 I2 # 7 I8 #25 J2 # 8 J8 #26 K2 # 9 K8 #27 I3 #10 I9 #28 J3 #11 J9 #29 K3 #12 K9 #30 I4 #13 I10 #31 J4 #14 J10 #32 K4 #15 K10 #33 I5 #16 J5 #17 K5 #18
(Note 1) Subscripts 1 to 10 for I, J, and K indicate the order of the specified command sets. They are not required to specify instructions.
(1) Local variables in subprograms can be defined by means of the designation
during macro call.
Main program
Refer to the local variables and control the movement, etc.
Subprogram (9900)
Local variables set by argument
Local variable data table
G65 P9900 A60. S100. F800; M02;
To subprogram
G91 G01 X [#19COS [#1] ] Y [#19SIN [#1] ] F#9;
M99;
A(#1)= 60.000 F(#9)= 800 S(#19)= 100.000
13. Program Support Functions 13.5 User Macro Specifications
315
(2) The local variables can be used freely in that subprogram.
Main program Subprogram (1)
Local variables set by argument
Local variable data table
The local variables can be changed in the subprogram.
G65 P1 A100. B50. J10. F500;
#30=FUP [#2/#5/2] ; #5=#2/#30/2 ; M98 H100 L#30 ; X#1 ; M99 ; N100 G1 X#1 F#9 ; Y#5 ; X-#1 ; Y#5 ; M99 ;
A (#1) 100.000 B (#2) 50.000 F (#9) 500 J (#5) 10.000 8.333 (#30) 3
Example of front surface milling
To subprogram
The local variables can be changed in the subprogram.
J
A
B
In the front surface milling example, argument J is programmed as the milling pitch 10.mm.
However, this is changed to 8.333mm to create an equal interval pitch. The results of the No. of reciprocation data calculation is set in local variable #30.
13. Program Support Functions 13.5 User Macro Specifications
316
(3) Local variables can be used independently on each of the macro call levels (4 levels). Local variables are also provided independently for the main program (macro level 0). Arguments cannot be used for the level 0 local variables.
Main (level 0) O1 (macro level 1) O10 (macro level 2) O100 (macro level 3) #1=0.1 #2=0.2 #3=0.3;
G65 P1A1. B2. C3.;
M02;
G65 P10A10. B20. C30.;
M99;
G65 P100A100. B200.;
M99;
M99;
Local variables (0) #1 0.100 #2 0.200 #3 0.300 #32
Local variables (1) A (#1) 1.000 B (#2) 2.000 C (#3) 3.000 D (#7) Z(#26) #32
Local variables (2) A (#1) 10.000 B (#2) 20.000 C (#3) 30.000 D (#7) Z(#26) #32
Local variables (3) A (#1) 100.000 B (#2) 200.000 C (#3) Z(#26) #32
The status of the local variables appear on the setting and display unit. Refer to the Operation Manual for details.
13. Program Support Functions 13.5 User Macro Specifications
317
Macro interface inputs (#1000 to #1035, #1200 to #1295) : PLC NC
The status of the interface input signals can be ascertained by reading out the values of variable numbers #1000 to #1035, #1200 to #1295. A variable value which has been read out can be only one of 2 values: 1 or 0 (1: contact closed, 0: contact open). All the input signals from #1000 to #1031 can be read at once by reading out the value of variable number #1032. Similarly, the input signals #1200 to #1231, #1232 to #1263, and #1264 to #1295 can be read by reading the values of the variable numbers #1033 to #1035. Variable numbers #1000 to #1035, #1200 to #1295 are for readout only, and cannot be placed in the left side member of their arithmetic formula. Input here refers to input to the control unit. System variable
No. of points
Interface input signal
System variable
No. of points
Interface input signal
#1000 #1001 #1002 #1003 #1004 #1005 #1006 #1007 #1008 #1009 #1010 #1011 #1012 #1013 #1014 #1015
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6436 bit 0 Register R6436 bit 1 Register R6436 bit 2 Register R6436 bit 3 Register R6436 bit 4 Register R6436 bit 5 Register R6436 bit 6 Register R6436 bit 7 Register R6436 bit 8 Register R6436 bit 9 Register R6436 bit 10 Register R6436 bit 11 Register R6436 bit 12 Register R6436 bit 13 Register R6436 bit 14 Register R6436 bit 15
#1016 #1017 #1018 #1019 #1020 #1021 #1022 #1023 #1024 #1025 #1026 #1027 #1028 #1029 #1030 #1031
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6437 bit 0 Register R6437 bit 1 Register R6437 bit 2 Register R6437 bit 3 Register R6437 bit 4 Register R6437 bit 5 Register R6437 bit 6 Register R6437 bit 7 Register R6437 bit 8 Register R6437 bit 9
Register R6437 bit 10 Register R6437 bit 11 Register R6437 bit 12 Register R6437 bit 13 Register R6437 bit 14 Register R6437 bit 15
System variable
No. of points
Interface input signal
#1032 #1033 #1034 #1035
32 32 32 32
Register R6436, R6437 Register R6438, R6439 Register R6440, R6441 Register R6442, R6443
13. Program Support Functions 13.5 User Macro Specifications
318
System variable
No. of points
Interface input signal
System variable
No. of points
Interface input signal
#1200 #1201 #1202 #1203 #1204 #1205 #1206 #1207 #1208 #1209 #1210 #1211 #1212 #1213 #1214 #1215
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6438 bit 0 Register R6438 bit 1 Register R6438 bit 2 Register R6438 bit 3 Register R6438 bit 4 Register R6438 bit 5 Register R6438 bit 6 Register R6438 bit 7 Register R6438 bit 8 Register R6438 bit 9
Register R6438 bit 10 Register R6438 bit 11 Register R6438 bit 12 Register R6438 bit 13 Register R6438 bit 14 Register R6438 bit 15
#1216 #1217 #1218 #1219 #1220 #1221 #1222 #1223 #1224 #1225 #1226 #1227 #1228 #1229 #1230 #1231
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6439 bit 0 Register R6439 bit 1 Register R6439 bit 2 Register R6439 bit 3 Register R6439 bit 4 Register R6439 bit 5 Register R6439 bit 6 Register R6439 bit 7 Register R6439 bit 8 Register R6439 bit 9
Register R6439 bit 10 Register R6439 bit 11 Register R6439 bit 12 Register R6439 bit 13 Register R6439 bit 14 Register R6439 bit 15
System variable
No. of points
Interface input signal
System variable
No. of points
Interface input signal
#1232 #1233 #1234 #1235 #1236 #1237 #1238 #1239 #1240 #1241 #1242 #1243 #1244 #1245 #1246 #1247
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6440 bit 0 Register R6440 bit 1 Register R6440 bit 2 Register R6440 bit 3 Register R6440 bit 4 Register R6440 bit 5 Register R6440 bit 6 Register R6440 bit 7 Register R6440 bit 8 Register R6440 bit 9
Register R6440 bit 10 Register R6440 bit 11 Register R6440 bit 12 Register R6440 bit 13 Register R6440 bit 14 Register R6440 bit 15
#1248 #1249 #1250 #1251 #1252 #1253 #1254 #1255 #1256 #1257 #1258 #1259 #1260 #1261 #1262 #1263
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6441 bit 0 Register R6441 bit 1 Register R6441 bit 2 Register R6441 bit 3 Register R6441 bit 4 Register R6441 bit 5 Register R6441 bit 6 Register R6441 bit 7 Register R6441 bit 8 Register R6441 bit 9
Register R6441 bit 10 Register R6441 bit 11 Register R6441 bit 12 Register R6441 bit 13 Register R6441 bit 14 Register R6441 bit 15
13. Program Support Functions 13.5 User Macro Specifications
319
System variable
No. of points
Interface input signal
System variable
No. of points
Interface input signal
#1264 #1265 #1266 #1267 #1268 #1269 #1270 #1271 #1272 #1273 #1274 #1275 #1276 #1277 #1278 #1279
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6442 bit 0 Register R6442 bit 1 Register R6442 bit 2 Register R6442 bit 3 Register R6442 bit 4 Register R6442 bit 5 Register R6442 bit 6 Register R6442 bit 7 Register R6442 bit 8 Register R6442 bit 9
Register R6442 bit 10 Register R6442 bit 11 Register R6442 bit 12 Register R6442 bit 13 Register R6442 bit 14 Register R6442 bit 15
#1280 #1281 #1282 #1283 #1284 #1285 #1286 #1287 #1288 #1289 #1290 #1291 #1292 #1293 #1294 #1295
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6443 bit 0 Register R6443 bit 1 Register R6443 bit 2 Register R6443 bit 3 Register R6443 bit 4 Register R6443 bit 5 Register R6443 bit 6 Register R6443 bit 7 Register R6443 bit 8 Register R6443 bit 9
Register R6443 bit 10 Register R6443 bit 11 Register R6443 bit 12 Register R6443 bit 13 Register R6443 bit 14 Register R6443 bit 15
Macro interface outputs (#1100 to #1135, #1300 to #1395) NC PLC
The interface output signals can be sent by substituting values in variable numbers #1100 to #1135, #1300 to #1395. An output signal can be only 0 or 1. All the output signals from #1100 to #1131 can be sent at once by substituting a value in variable number #1132. Similarly, the output signals #1300 to #1311, #1332 to #1363, and #1364 to #1395 can be sent by assigning values to the variable numbers #1133 to #1135. (20 to 231) The status of the writing and output signals can be read in order to offset the #1100 to #1135, #1300 to #1395 output signals. Output here refers to the output from the NC side.
System variable
No. of points
Interface output signal
System variable
No. of points
Interface output signal
#1100 #1101 #1102 #1103 #1104 #1105 #1106 #1107 #1108 #1109 #1110 #1111 #1112 #1113 #1114 #1115
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6372 bit 0 Register R6372 bit 1 Register R6372 bit 2 Register R6372 bit 3 Register R6372 bit 4 Register R6372 bit 5 Register R6372 bit 6 Register R6372 bit 7 Register R6372 bit 8 Register R6372 bit 9
Register R6372 bit 10 Register R6372 bit 11 Register R6372 bit 12 Register R6372 bit 13 Register R6372 bit 14 Register R6372 bit 15
#1116 #1117 #1118 #1119 #1120 #1121 #1122 #1123 #1124 #1125 #1126 #1127 #1128 #1129 #1130 #1131
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6373 bit 0 Register R6373 bit 1 Register R6373 bit 2 Register R6373 bit 3 Register R6373 bit 4 Register R6373 bit 5 Register R6373 bit 6 Register R6373 bit 7 Register R6373 bit 8 Register R6373 bit 9
Register R6373 bit 10 Register R6373 bit 11 Register R6373 bit 12 Register R6373 bit 13 Register R6373 bit 14 Register R6373 bit 15
13. Program Support Functions 13.5 User Macro Specifications
320
System variable
No. of points
Interface output signal
#1132 #1133 #1134 #1135
32 32 32 32
Register R6372, R6373 Register R6374, R6375 Register R6376, R6377 Register R6378, R6379
System variable
No. of points
Interface output signal
System variable
No. of points
Interface output signal
#1300 #1301 #1302 #1303 #1304 #1305 #1306 #1307 #1308 #1309 #1310 #1311 #1312 #1313 #1314 #1315
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6374 bit 0 Register R6374 bit 1 Register R6374 bit 2 Register R6374 bit 3 Register R6374 bit 4 Register R6374 bit 5 Register R6374 bit 6 Register R6374 bit 7 Register R6374 bit 8 Register R6374 bit 9
Register R6374 bit 10 Register R6374 bit 11 Register R6374 bit 12 Register R6374 bit 13 Register R6374 bit 14 Register R6374 bit 15
#1316 #1317 #1318 #1319 #1320 #1321 #1322 #1323 #1324 #1325 #1326 #1327 #1328 #1329 #1330 #1331
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6375 bit 0 Register R6375 bit 1 Register R6375 bit 2 Register R6375 bit 3 Register R6375 bit 4 Register R6375 bit 5 Register R6375 bit 6 Register R6375 bit 7 Register R6375 bit 8 Register R6375 bit 9
Register R6375 bit 10 Register R6375 bit 11 Register R6375 bit 12 Register R6375 bit 13 Register R6375 bit 14 Register R6375 bit 15
System variable
No. of points
Interface output signal
System variable
No. of points
Interface output signal
#1332 #1333 #1334 #1335 #1336 #1337 #1338 #1339 #1340 #1341 #1342 #1343 #1344 #1345 #1346 #1347
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6376 bit 0 Register R6376 bit 1 Register R6376 bit 2 Register R6376 bit 3 Register R6376 bit 4 Register R6376 bit 5 Register R6376 bit 6 Register R6376 bit 7 Register R6376 bit 8 Register R6376 bit 9
Register R6376 bit 10 Register R6376 bit 11 Register R6376 bit 12 Register R6376 bit 13 Register R6376 bit 14 Register R6376 bit 15
#1348 #1349 #1350 #1351 #1352 #1353 #1354 #1355 #1356 #1357 #1358 #1359 #1360 #1361 #1362 #1363
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6377 bit 0 Register R6377 bit 1 Register R6377 bit 2 Register R6377 bit 3 Register R6377 bit 4 Register R6377 bit 5 Register R6377 bit 6 Register R6377 bit 7 Register R6377 bit 8 Register R6377 bit 9
Register R6377 bit 10 Register R6377 bit 11 Register R6377 bit 12 Register R6377 bit 13 Register R6377 bit 14 Register R6377 bit 15
13. Program Support Functions 13.5 User Macro Specifications
321
System variable
No. of points
Interface output signal
System variable
No. of points
Interface output signal
#1364 #1365 #1366 #1367 #1368 #1369 #1370 #1371 #1372 #1373 #1374 #1375 #1376 #1377 #1378 #1379
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6378 bit 0 Register R6378 bit 1 Register R6378 bit 2 Register R6378 bit 3 Register R6378 bit 4 Register R6378 bit 5 Register R6378 bit 6 Register R6378 bit 7 Register R6378 bit 8 Register R6378 bit 9
Register R6378 bit 10 Register R6378 bit 11 Register R6378 bit 12 Register R6378 bit 13 Register R6378 bit 14 Register R6378 bit 15
#1380 #1381 #1382 #1383 #1384 #1385 #1386 #1387 #1388 #1389 #1390 #1391 #1392 #1393 #1394 #1395
1 1 1 1 1 1 1 1 1 1 1 1 1 1 1 1
Register R6379 bit 0 Register R6379 bit 1 Register R6379 bit 2 Register R6379 bit 3 Register R6379 bit 4 Register R6379 bit 5 Register R6379 bit 6 Register R6379 bit 7 Register R6379 bit 8 Register R6379 bit 9
Register R6379 bit 10 Register R6379 bit 11 Register R6379 bit 12 Register R6379 bit 13 Register R6379 bit 14 Register R6379 bit 15
(Note 1) The last values of the system variables #1100 to #1135, #1300 to #1395 sent are retained as 1 or 0. (They are not cleared even with resetting.)
(Note 2) The following applies when any number except 1 or 0 is substituted into #1100 to #1131, #1300 to #1395. is treated as 0. Any number except 0 and is treated as 1. Any value less than 0.00000001 is indefinite.
13. Program Support Functions 13.5 User Macro Specifications
322
Output signal
M ac
ro in
st ru
ct io
ns
#1000
#1031
Input signal #1032 (R6436, R6437)
#1200
#1231
#1033 (R6438, R6439)
#1232
#1263
#1034 (R6440, R6441)
#1264
#1295
#1035 (R6442, R6443)
#1100
#1131
#1132 (R6372, R6373)
#1300
#1331
#1133 (R6374, R6375)
#1332
#1363
#1134 (R6376, R6377)
#1364
#1395
#1135 (R6378, R6379)
13. Program Support Functions 13.5 User Macro Specifications
323
Tool compensation
Tool data can be read and set using the variable numbers.
Variable number range Type 1 Type 2 #10001 to #10000 + n #2001 to #2000 + n (Length dimension) #11001 to #11000 + n #2201 to #2200 + n (Length wear)
#16001 to #16000 + n #2401 to #2400 + n (Radius dimension) #17001 to #17000 + n #2601 to #2600 + n (Radius wear)
«n» in the table indicates the tool No. The maximum value of «n» matches the number of tool offset sets. Numbers in the #10000 order have the equivalent function to that in the #2000 order, however, the maximum value of «n» for #2000 order is «200». When the number of tool offset sets is larger than «200», use the variables of #10000 order. The tool compensation data are configured as data with a decimal point in the same way as for other variables. Consequently, programming as «#10001 = 1000;» results the setting «1000.000» in the tool compensation data.
#101=1000; #10001=#101; #102=#10001;
#101=1000.0 #102=1000.0
H1=1000.000After
execution
Programming example Common variables Tool compensation data
(Example 1) Calculation and tool offset data setting
# 1
H 1
#5063
Sensor
G31
G00
Reference position return Tool change (spindle T01) Start point memory Rapid traverse to safety position Skip measurement Measured distance calculation and tool compensation data setting
G28 Z0 T01 ;
M06 ;
#1=#5003 ;
G00 Z-500. ;
G31 Z-100. F100;
#10001=#5063-#1 ;
(Note) In this example, no consideration is given to the delay in the skip sensor signal. #5003 is the Z axis start point position and #5063 is the Z axis skip coordinates, and
indicated is the position at which the skip signal is input while G31 is being executed.
13. Program Support Functions 13.5 User Macro Specifications
324
Workpiece coordinate system offset
By using variable numbers #5201 to #532n, it is possible to read out the workpiece coordinate system offset data or to substitute values. (Note) The number of axes which can be controlled differs according to the specifications.
The last digit of the variable No. corresponds to the control axis No. Axis No.
Axis name Axis 1 Axis 2 Axis 3 Axis 4 . . Axis n Remarks
External workpiece offset #5201 #5202 #5203 #5204 . . #520n External workpiece offset
specifications are required. G54 #5221 #5222 #5223 #5224 . . #522n G55 #5241 #5242 #5243 #5244 . . #524n G56 #5261 #5262 #5263 #5264 . . #526n G57 #5281 #5282 #5283 #5284 . . #528n G58 #5301 #5302 #5303 #5304 . . #530n G59 #5321 #5322 #5323 #5324 . . #532n
N1 G28 X0 Y0 Z0 ; N2 #5221=-20. #5222=-20. ; N3 G90 G00 G54 X0 Y0 ; N10 #5221=-90. #5222=-10. ; N11 G90 G00 G54 X0Y0 ; M02 ;
N100 #5221=#5221+#5201 ; #5222=#5222+#5202 ; #5241=#5241+#5201 ; #5242=#5242+#5202 ; #5201=0 #5202=0;
(Example 1)
External workpiece offset (Example 2)
G54 workpiece coordinate system defined by N10 G54 workpiece
coordinate system defined by N2
Base machine coordinate system
Base machine coordinate system
-90. -20.
-20. -10.
N1
N3
W1 W1 N11
W1 (G54) W2 (G55)
M
W2 (G55) W1 (G54)
M
G55 G54
Coordinate system before change
Coordinate system after change
G54 G55
This is an example where the external workpiece offset values are added to the workpiece coordinate (G54, G55) system offset values without changing the position of the workpiece coordinate systems.
13. Program Support Functions 13.5 User Macro Specifications
325
Alarm (#3000)
The NC system can be forcibly set to the alarm state by using variable number #3000.
Format
#3000 = 70 (CALL#PROGRAMMER#TEL#530) :
Any alarm number from 1 to 9999 can be specified. The alarm message must be less than 31 characters long. «NC alarm 3 (program error)» signal will be output. The «P277» user macro alarm message appears in the column on diagnosis screen 1 while the alarm number and alarm message CALL #PROGRAMMER #TEL#530 is indicated in the .
Example of program (alarm when #1 = 0) IF [#1 NE 0] GOTO 100 ; #3000=70 (CALL#PROGRAMMER#TEL#530) ; N100
P277 : Macro alarm message
CALL#PROGRAMMER#TEL#530 70
Stops with NC alarm
(Note 1) Alarm number 0 is not displayed and any number exceeding 9999 cannot be indicated. (Note 2) The characters following the first alphabet letter in the right member is treated as the
alarm message. Therefore, a number cannot be designated as the first character of an alarm message. It is recommended that the alarm messages be enclosed in round parentheses.
70 : Alarm number CALL#PROGRAMMER#TEL#530 : Alarm message
13. Program Support Functions 13.5 User Macro Specifications
326
Integrating (run-out) time (#3001, #3002)
The integrating (run-out) time can be read during automatic operation or automatic start or values can be substituted by using variable numbers #3001 and #3002.
Type Variable number Unit
Contents when power is switched
on
Initialization of contents Count condition
Integrating (run-out) time 1 3001 At all times while
power is ON Integrating (run-out) time 2 3002
ms Same as when power is switched off
Value substituted for variable
In-automatic start
The integrating run time returns to zero in about 2.44 1011 ms (approximately 7.7 years).
G65P9010 T ms; (allowable
time) To subprogram
Local variableEntered in local variable #20
Allowable time portion : DO1-END is repeated and when allowable time is reached, operations jumps to M99.
T#20
#3001=0 ; WHILE [#3001LE#20] DO1 ; END1 : M99 ;
O9010
Suppression of single block stop and miscellaneous function finish signal waiting
By substituting the values below in variable number #3003, it is possible to suppress single block stop in the subsequent blocks or to advance to the next block without waiting for the miscellaneous function (M, S, T, B) finish (FIN) signal.
#3003 Single block stop Miscellaneous function finish signal 0 Not suppressed Awaited 1 Suppressed Awaited 2 Not suppressed Not awaited 3 Suppressed Not awaited
(Note 1) #3003 is cleared to zero by NC reset.
13. Program Support Functions 13.5 User Macro Specifications
327
Feed hold, feedrate override, G09 valid/invalid
By substituting the values below in variable number #3004, it is possible to make the feed hold, feedrate override and G09 functions either valid or invalid in the subsequent blocks.
Bit 0 Bit 1 Bit 2 #3004 Contents (value) Feed hold Feedrate override G09 check
0 Valid Valid Valid 1 Invalid Valid Valid 2 Valid Invalid Valid 3 Invalid Invalid Valid 4 Valid Valid Invalid 5 Invalid Valid Invalid 6 Valid Invalid Invalid 7 Invalid Invalid Invalid
(Note 1) Variable number #3004 is set to zero by NC reset. (Note 2) The functions are valid when the above bits are 0 and invalid when they are 1. (Note 3) When the feed hold is set to invalid with #3004, the following will occur when the feed hold
switch is pressed. During thread cutting, block stop will be carried out at the end of the next block of the
block where thread cutting is completed. During tapping with tap cycle, block stop will be carried out after the operation of R point
return. In the case other than above, block stop will be carried out after termination of the
currently executing block.
Message display and stop
By using variable number #3006, the execution is stopped after the previous block has been executed and, if message display data have been commanded, then the corresponding message will be indicated on the operator message area.
Format
#3006 = 1 ( TAKE FIVE ) :
1 Fixed value (Nothing is displayed if a value other than 1 is set.)
TAKE FIVE Message The message should not be longer than 31 characters and it should be enclosed within round ( ) parentheses.
Mirror image
By reading variable number #3007, it is possible to ascertain the status of mirror image at a particular point in time for each axis. The axes correspond to the bits of #3007. When the bits are 0, it means that the mirror image function is not valid; when they are 1, it means that it is valid.
#3007
Bit 15 14 13 12 11 10 9 8 7 6 5 4 3 2 1 0 nth axis 6 5 4 3 2 1
13. Program Support Functions 13.5 User Macro Specifications
328
G command modals
Using variable numbers #4001 to #4021, it is possible to read the G modal commands which have been issued up to the block immediately before. Similarly, it is possible to read the modals in the block being executed with variable numbers #4201 to #4221.
Variable number Pre-read
block Execution
block Function
#4001 #4201 Interpolation mode : G00:0, G01:1, G02:2, G03:3, G33:33
#4002 #4202 Plane selection : G17:17, G18:18, G19:19 #4003 #4203 Absolute/incremental : G90:90, G91:91 #4004 #4204 No variable No. #4005 #4205 Feed designation : G94:94, G95:95 #4006 #4206 Inch/metric : G20:20, G21/21 #4007 #4207 Tool nose R compensation : : G40:40, G41:41, G42:42 #4008 #4208 Tool length compensation : G43:43, G44:44, G49:49
#4009 #4209 Canned cycle : G80:80, G73 to 74, G76:76, G81 to G89:81 to 89
#4010 #4210 Return level : G98:98, G99:99 #4011 #4211 #4012 #4212 Workpiece coordinate system : G54 to G59:54 to 59
#4013 #4213 Acceleration/deceleration : G61 to G64:61 to 64, G61.1:61.1
#4014 #4214 Macro modal call : G66:66, G66.1:66.1, G67:67 #4015 #4215 #4016 #4216 #4017 #4217 Constant surface speed control : G96:96, G97:97 #4018 #4218 No variable No. #4019 #4219 Mirror image : G50.1:50.1, G51.1:51.1 #4020 #4220 #4021 #4221 No variable No.
(Example) G28 X0 Y0 Z0 ; G90 G1 X100. F1000; G91 G65 P300 X100. Y100.; M02; O300;
#1 = #4003; Group 3G modal (pre-read) #1 = 91.0 #2 = #4203; Group 3G modal (now being executed) #2 = 90.0 G#1 X#24 Y#25; M99; %
13. Program Support Functions 13.5 User Macro Specifications
329
Other modals
Using variable numbers #4101 to #4120, it is possible to read the model commands assigned up to the block immediately before. Similarly, it is possible to read the modals in the block being executed with variable numbers #4301 to #4320.
Variable number Variable number Pre-read Execution
Modal information Pre-read Execution
Modal information
#4101 #4301 #4111 #4311 Tool length compensation No. H
#4102 #4302 #4112 #4312 #4103 #4303 #4113 #4313 Miscellaneous function M #4104 #4304 #4114 #4314 Sequence number N
#4105 #4305 #4115 #4315 Program number O (Note 1)
#4106 #4306 #4116 #4316
#4107 #4307 Tool radius compensation No. D #4117 #4317
#4108 #4308 #4118 #4318 #4109 #4309 Feedrate F #4119 #4319 Spindle function S #4110 #4310 #4120 #4320 Tool function T
(Note 1) The programs are registered as files. When the program No. (file name) is read with #4115, #4315, the character string will be converted to a value.
(Example 1) The file name «123» is the character string 031, 032, 033, so the value will be
(031-030)*100 + (032-030)*10 + (033-030) = 123.0. Note that if the file name contains characters other than numbers, it will be «blank».
(Example 2) If the file name is «123ABC», it contains characters other than numbers; so, the
result will be «blank».
13. Program Support Functions 13.5 User Macro Specifications
330
Position information
Using variable numbers #5001 to #5104, it is possible to read the servo deviation amounts, tool position compensation amount, skip coordinates, workpiece coordinates, machine coordinates and end point coordinates in the block immediately before.
Axis No.
Position information
1 2 3 4 n
Remarks (reading during
movement)
End point coordinate of block immediately before #5001 #5002 #5003 #5004 #5000+n Yes
Machine coordinate #5021 #5022 #5023 #5024 #5020+n No Workpiece coordinate #5041 #5042 #5043 #5044 #5040+n No Skip coordinate #5061 #5062 #5063 #5064 #5060+n Yes Tool position compensation amount #5081 #5082 #5083 #5084 #5080+n No
Servo deviation amount #5101 #5102 #5103 #5104 #5100+n Yes Start point coordinate of block with a macro interrupt
#5121 #5122 #5123 #5124 #5120+n Yes
End point coordinate of block with a macro interrupt
#5141 #5142 #5143 #5144 #5140+n Yes
(Note 1) The number of axes which can be controlled differs according to the specifications. (Note 2) The last digit of the variable No. corresponds to the control axis No.
13. Program Support Functions 13.5 User Macro Specifications
331
Basic machine coordinate system
Workpiece coordinate system
[End point coordinates]
[Workpiece coordinates]
[Machine coordinates]
Workpiece coordinate system
Machine coordinate system
W
M
M
W
Read command
G01
G00
(1) The positions of the end point coordinates and skip coordinates are positions in the workpiece
coordinate system. (2) The end point coordinates, skip coordinates and servo deviation amounts can be read even
during movement. However, it must first be checked that movement has stopped before reading the machine coordinates and the workpiece coordinates.
(3) The position where the skip signal is turned ON in the G31 block is indicated for the skip coordinates. The end point position is indicated when the skip signal has not been turned ON. (For further details, refer to the section on tool length measurement.)
Skip coordinates
Gauge, etc. Read command
13. Program Support Functions 13.5 User Macro Specifications
332
(4) The tool nose position where the tool compensation and other such factors are not considered
is indicated as the end point position. The tool reference position with consideration given to tool compensation is indicated for the machine coordinates, workpiece coordinates and skip coordinates.
Skip signal
F (feedrate)
[Input coordinates of skip signal]
[Workpiece coordinates]
Workpiece coordinate system
Machine coordinate system
[Machine coordinates]
G31
W
M
For » «, check stop and then proceed to read. For » «, reading is possible during movement.
The position of the skip signal input coordinates is the position in the workpiece coordinate system. The coordinates in variable numbers #5061 to #5064 memorize the moments when the skip input signal during movement was input and so they can be read at any subsequent time. For further details, reference should be made to the section on the skip function.
13. Program Support Functions 13.5 User Macro Specifications
333
(Example 1) Example of workpiece position measurement
An example to measure the distance from the measured reference position to the workpiece edge is shown below.
G65 P9031 X100. Y100. Z-10. F200;
F(#9) 200 X(#24)100.000 Y(#25)100.000 Z(#26) -10.000
#101 87.245 #102 87.245 #103 123.383
N1 #180=#4003; N2 #30=#5001 #31=#5002; N3 G91 G01 Z#26 F#9; N4 G31 X#24 Y#25 F#9; N5 G90 G00 X#30 Y#31; N6 #101=#30-#5061 #102=#31-#5062; N7 #103=SQR [#101#101+#102*#102] ; N8 G91 G01Z-#26; N9 IF [#180 EQ 91] GOTO 11; N10 G90; N11 M99;
To subprogram
Main program
Argument O9031
Start point
Skip input
N3 N4
N5 N8 #103 #102
#101 X
Z
Y
#101 X axis measurement amount N1 G90/G91 modal recording #102 X axis measurement amount N2 X, Y start point recording #103 Measurement linear segment N3 Z axis entry amount amount N4 X, Y measurement (Stop at skip input) #5001 X axis measurement start point N5 Return to X, Y start point #5002 Y axis measurement start point N6 X, Y measurement incremental value calculation N7 Measurement linear segment calculation #5061 X axis skip input point N8 Z axis escape #5062 Y axis skip input point N9, N10 G90/G91 modal return N11 Subprogram return
(Example 2) Reading of skip input coordinates
-Y
-50
-75
-100
N1 G91 G28 X0 Y0; N2 G90 G00 X0 Y0; N3 X0Y-100.; N4 G31 X-150. Y-50. F80; N5 #111=#5061#112=#5062; N6 G00 Y0; N7 G31 X0; N8 #121=#5061#122=#5062; N9 M02;
-150 -75 -25 Y X-X
Skip signal
#111 = 75. + #112 = 75. + #121 = 25. + #122 = 75. + is the error caused by response delay. (Refer to the section on the skip function for details.) #122 is the N4 skip signal input coordinates as there is no Y command at N7.
13. Program Support Functions 13.5 User Macro Specifications
334
Variable name setting and quotation
Any name (variable name) can be given to common variables #500 to #519. It must be composed of not more than 7 alphanumerics and it must begin with a letter. Do not use «#» in variable names. It causes an alarm when the program is executed.
Format
SETVN n [ NAME1, NAME2, ] : n : Head number of variable to be named NAME1 : #n name (variable name) NAME2 : #n + 1 name (variable name)
Variable names are separated by a comma (,).
Detailed description (1) Once variable names have been set, they will not be cleared even when the power is switched
off. (2) Variables in programs can be quoted by their variable names. In cases like this, the variables
should be enclosed in square parentheses. (Example 1) G01X [#POINT1] ;
[#NUMBER] = 25 ;
(3) The variable numbers, data and variable names appear on the screen of the setting and display unit.
(Example 2) Program …… SETVN500 [A234567, DIST, TOOL25] ;
[Common variables] #500 -12345.678 A234567
#501 5670.000 DIST
#502 -156.500 TOOL25
#518 10.000 NUMBER
Common variable #(502) Data (-156.5) Name (TOOL25)
(Note) At the head of the variable name, do not use the characters determined by the NC for use in arithmetic commands, etc. (e.g. SIN, COS).
13. Program Support Functions 13.5 User Macro Specifications
335
Number of workpiece machining times
The number of workpiece machining times can be read using variables #3901 and #3902. By substituting a value in these variables, the number of workpiece machining times can be changed.
Type Variable No. Data setting range Number of workpiece machining times #3901
Maximum workpiece value #3902
0 to 999999
(Note) Always substitute a positive value for the number of workpiece machining times.
Coordinate rotation parameter
The following variables can be read by the system variables of the variable command. Note that writing is not possible onto these variables.
Variable No. Description
#30060 Control axis No. on the coordinate rotation plane (horizontal axis)
#30061 Control axis No. on the coordinate rotation plane (vertical axis)
#30062 Coordinate rotation center (horizontal axis) #30063 Coordinate rotation center (vertical axis) #30064 Coordinate rotation angle
#30065 SIN data for the coordinate rotation angle [SIN(Coordinate rotation angle)]
#30066 COS data for the coordinate rotation angle [COS(Coordinate rotation angle)]
#30067 Coordinate rotation vector (horizontal axis) #30068 Coordinate rotation vector (vertical axis)
Reverse run information
Variable number Usage Description Range
#31100 Number of available blocks for reverse run
+1 added number of the blocks that retained the reverse run information while the Reverse run control mode signal was ON
0 to 201
#31101 Counter of available blocks for reverse run
Number of available blocks for reverse run (value of #31100) when the Reverse run signal turned ON to start. Turns 0 when the forward run has been executed for all the blocks. Shows 0 in the normal operation.
0 to 201
13. Program Support Functions 13.5 User Macro Specifications
336
Tool life management
(1) Definition of variable numbers
(a) Designation of group No. #60000
The tool life management data group No. to be read with #60001 to #64700 is designated by substituting a value in this variable. If a group No. is not designated, the data of the group registered first is read. This is valid until reset.
(b) Tool life management system variable No. (Read)
#60001 to #64700
# ? ? ? ? ?
+ Variable No. or data type Data class 6: Tool life management
(c) Details of data classification
Data class M System L System Remarks 00 For control For control Refer to following types 05 Group No. Group No. Refer to registration No. 10 Tool No. Tool No. Refer to registration No. 15 Tool data flag Method Refer to registration No. 20 Tool status Status Refer to registration No. 25 Life data Life time/No. of times Refer to registration No.
30 Usage data Usage time/No. of times Refer to registration No.
35 Tool length compensation data — Refer to registration No.
40 Tool radius compensation data — Refer to registration No.
45 Auxiliary data — Refer to registration No. The group No., L System method, and life data are common for the group.
(d) Registration No.
M system 1 to 200 L system 1 to 16
13. Program Support Functions 13.5 User Macro Specifications
337
(e) Data type
Type M System L System Remarks
1 Number of registered tools
Number of registered tools
2 Life current value Life current value 3 Tool selected No. Tool selected No.
4 Number of remaining registered tools
Number of remaining registered tools
5 Signal being executed Signal being executed
6 Cutting time cumulative value (minute)
Cutting time cumulative value (minute)
7 Life end signal Life end signal
8 Life prediction signal Life prediction signal
Variable No. Item Type Details Data range
60001 Number of registered tools
Common to system
Total number of tools registered in each group. 0 to 200
60002 Life current value Usage time/No. of uses of tool being used. Spindle tool usage data or usage data for tool in use (#60003).
0 to 4000 minutes 0 to 9999 times
60003 Tool selected No. Registration No. of tool being used. Spindle tool registration No. (If spindle tool is not data of the designated group, ST:1 first tool, or if ST:1 is not used, the first tool of ST:0. When all tools have reached their lives, the last tool.)
0 to 200
60004 Number of remaining registered tools
No. of first registered tool that has not reached its life.
0 to 200
60005 Signal being executed
«1» when this group is used in program being executed. «1» when spindle tool data group No. and designated group No. match.
0/1
60006 Cutting time cumulative value (minute)
Indicates the time that this group is used in the program being executed.
(Not used)
60007 Life end signal «1» when lives of all tools in this group have been reached. «1» when all tools registered in designated group reach lives.
0/1
60008 Life prediction signal
For each group (Designate group No. #60000)
«1» when new tool is selected with next command in this group. «1» when there are no tools in use (ST: 1) while there is an unused tool (ST: 0) in the specified group.
0/1
13. Program Support Functions 13.5 User Macro Specifications
338
Variable No. Item Type Details Data range
60500 +***
Group No. This group’s No. 1 to 99999999
61000 +***
Tool No. Tool No. 1 to 99999999
61500 +***
Tool data flag Usage data count method, length compensation method, radius compensation method, etc., parameters. bit 0, 1 : Tool length compensation data
format bit 2, 3 : Tool radius compensation data
format 0: Compensation No. method 1: Incremental value compensation
amount method 2: Absolute value compensation
amount method bit 4, 5 : Tool life management method
0: Usage time 1: No. of mounts 2: No. of usages
0 to FF (H)
62000 +***
Tool status Tool usage state 0: Not used tool 1: Tool being used 2: Normal life tool 3: Tool error 1 4: Tool error 2
0 to 4
62500 +***
Life data Life time or No. of lives for each tool 0 to 4000 minutes 0 to 9999 times
63000 +***
Usage data Usage time or No. of uses for each tool 0 to 4000 minutes 0 to 9999 times
63500 +***
Tool length compensation data
Length compensation data set as compensation No., absolute value compensation amount or increment value compensation amount method.
Compensation No.: 0 to No. of tool compensation sets Absolute value compensation amount 99999.999 Increment value compensation amount 99999.999
64000 +***
Tool radius compensation data
Radius compensation data set as compensation No., absolute value compensation amount or increment value compensation amount method.
Compensation No.: 0 to No. of tool compensation sets Absolute value compensation amount 99999.999 Increment value compensation amount 99999.999
64500 +***
Auxiliary data
Each group/ registration No. (Designate the group No. #60000 and registration No. *** .) Note the group No., method and life are common for the groups.
Spare data 0 to 65535
13. Program Support Functions 13.5 User Macro Specifications
339
Example of program for tool life management
(1) Normal commands
#101 = #60001 ; ………….Reads the number of registered tools. #102 = #60002 ; ………….Reads the life current value. #103 = #60003 ; ………….Reads the tool selection No. #60000 = 10 ; ……………..Designates the group No. of the life data to be read. #104 = #60004 ; ………….Reads the remaining number of registered tools in group 10. #105 = #60005 ; ………….Reads the signal being executed in group 10. #111 = #61001 ; ………….Reads the group 10, #1 tool No. #112 = #62001 ; ………….Reads the group 10, #1 status. #113 = #61002 ; ………….Reads the group 10, #2 status. %
Designated program No. is valid until reset.
(2) When group No. is not designated.
#104 = #60004 ; ……….. Reads the remaining number of registered tools in the group registered first.
#111 = #61001 ; ……….. Reads the #1 tool No. in the group registered first. %
(3) When non-registered group No. is designated. (Group 9999 does not exist.)
#60000 = 9999 ; ……….. Designates the group No. #104 = #60004 ; ……….. #104 = -1.
(4) When registration No. not used is designated. (Group 10 has 15 tools) #60000 = 10 ; …………… Designates the group No. #111 = #61016 ; ……….. #101 = -1.
(5) When registration No. out of the specifications is designated.
#60000 = 10 ; #111 = #61017 ; ……….. Program error (P241)
(6) When tool life management data is registered with G10 command after group No. is
designated. #60000 = 10 ; ………Designates the group No. G10 L3 ; ……………….Starts the life management data registration. P10 LLn NNn ; ……..10 is the group No., Ln is the life per tool, Nn is the method. TTn ; …………………..Tn is the tool No. : G11 ; ………………….Registers the group 10 data with the G10 command. #111 = #61001 ; …..Reads the group 10, #1 tool No. G10 L3 ; ……………….Starts the life management data registration. P1 LLn NNn ; ……….1 is the group No., Ln is the life per tool, Nn is the method. TTn ; …………………..Tn is the tool No. : G11 ; ……………………Registers the life data with the G10 command. (The registered data is deleted.) #111 = 61001 ; …….Group 10 does not exist. #201 = 1.
The group 10 life data is registered.
The life data other than group 10 is registered.
13. Program Support Functions 13.5 User Macro Specifications
340
Precautions for tool life management
(1) If the tool life management system variable is commanded without designating a group No.,
the data of the group registered at the head of the registered data will be read. (2) If a non-registered group No. is designated and the tool life management system variable is
commanded, «-1» will be read as the data. (3) If an unused registration No. tool life management system variable is commanded, «-1» will be
read as the data. (4) Once commanded, the group No. is valid until NC reset.
13. Program Support Functions 13.5 User Macro Specifications
341
Reading the parameters
System data can be read in with the system variables.
(Note) These can be used only with some models.
Variable No. Application #100000 Parameter # designation #100001 Part system No. designation #100002 Axis No./spindle No. designation #100010 Parameter value read
The parameter values are read in with the following four blocks using these four system variables.
#100000 = 1001 ; ……… Designates the parameter #. #100001 = 1 ; …………… Designates the part system No. #100002 = 1 ; …………… Designates the axis No./spindle No. #100 = #100010 ; ……… Reads the parameter value. (1) Parameter # designation (#100000)
The parameter to be read in is designated by substituting the parameter # in this system variable. If the parameters are read without designating this number, the parameters will be read in the same manner as if the minimum parameter # (#1) is designated. Once designated, the setting is held until the parameter # is designated again or until it is reset. A program error (P39) will occur if a parameter # that does not exist is set.
(2) Part system No. designation (#100001)
Always set «0». When using the PLC axis, set «10».
(3) Axis/spindle No. designation (#100002)
(a) System variable for axis/spindle No. designation The axis No./spindle No. of the parameter to be read in is designated by substituting an index value in this system variable. This designation will be ignored when reading in parameters that are not for a specific axis or spindle. If the parameters are read without designating this number, the parameters will be read in the same manner as if the index value 1 (1st axis/1st spindle) is designated. Once designated, the setting is held until the index value is designated again or until it is reset. A program error (P39) will occur if an axis/spindle No. that does not exist is set.
(b) Index values
Index values Axis parameter Spindle parameter 1 1st axis 1st spindle 2 2nd axis 2nd spindle 3 3rd axis 3rd spindle 4 4th axis 4th spindle 5 5th axis — 6 6th axis —
13. Program Support Functions 13.5 User Macro Specifications
342
(4) Parameter read (#100010)
The designated parameter data is read with this system variable. The following data is read according to the parameter type.
Type Read data Value The values displayed on the Parameter screen are output. Text ASCII codes are converted into decimal values.
Example of programs for reading parameters
(1) To read the parameter [#1002 axisno (Number of axes)]
#100000 = 1002 ; …………………Designates [#1002]. #100001 = 0 ; #101 = #100010 ; …………………Reads the number of axes. #100001 = 5 ; ………………………Designates [5th part system]. (Program error (P39) occurs.) #100001 = 10 ; …………………….Designates [PLC axis]. #110 = #100010 ; …………………Reads the number of PLC axes.
(2) To read the parameter [#2037 G53ofs (#1 reference position)] [Conditions] <1st axis> <2nd axis> #2037 G53ofs 1000.000 200.000 #100002 = 1 ; ………………………Designates [1st axis]. #100000 = 2037 ; …………………Designates [#2037]. #101 = #100010 ; …………………Reads the [#1 reference position] for the 1st axis. (#101 = 100.000.) #100002 = 2 ; ………………………Designates [2nd axis]. #102 = #100010 ; …………………Reads the [#1 reference position] for the 2nd axis. (#102 = 200.000.)
(3) To read each parameter for each axis and spindle
#100002 = 1 ; ………………………Designates [1st spindle]. #100000 = 3001 ; …………………Designates [#3001]. #101 = #100010 ; …………………Reads the [#3001 slimt1 (Number of limit rotation gears 00)] for 1st spindle. #100000 = 3002 ; …………………Designates [#3002]. #102 = #100010 ; …………………Reads the [#3002 slimt2 (Number of limit rotation gears 01)] for 1st spindle. #100002 = 2 ; ………………………Designates [2nd spindle]. #100000 = 3001 ; …………………Designates [#3001]. #201 = #100010 ; …………………Reads the [#3001 slimt1 (Number of limit rotation gears 00)] for 2nd spindle. #100000 = 3002 ; …………………Designates [#3002]. #202 = #100010 ; …………………Reads the [#3002 slimt2 (Number of limit rotation gears 01)] for 2nd spindle
13. Program Support Functions 13.5 User Macro Specifications
343
Example of parameter read macro program
Q341 A_. Q_ . ; A_. …… Storage common variable Designates the common variable No. for storing the
data read in. Q_……. Parameter # designation For an axis/spindle parameter, designates the
axis/spindle No. with one digit after the decimal point.
#100000 = FIX [#17] ; ………. Designates parameter #. #100002 = FIX [#1710] MOD 10 ; ………. Designates axis/spindle No. #[#1] = #100010 ; ……….. Reads parameter data. M99 ;
Precautions for reading parameters
(1) The number of axes and spindles is the maximum number in the specifications determined by
the model.
(2) The inch/metric changeover function for the setting and display is valid even for the data read in.
13. Program Support Functions 13.5 User Macro Specifications
344
Reading PLC data
PLC data can be read in with the system variables.
(Note 1) These can be used only with some models.
(Note 2) The read devices are limited.
Variable No. Application #100100 Device type designation #100101 Device No. designation #100102 Number of read bytes designation #100103 Read bit designation #100110 PLC data read
The PLC data is read in with the following five blocks using these five system variables. #100100 = 1 ; …………Designates the device type. #100101 = 0 ; …………Designates the device No. #100102 = 1 ; …………Designates the number of bytes. #100103 = 2 ; …………Designates the bit. (Valid only when reading word device bits.) #100 = #100110 ; ……Reads in the PLC data. (1) Device designation (#100100)
(a) System variable for device designation The type of device to be read in can be designated by substituting the device designation value in this system variable. If the data is read without designating this number, the data will be read in the same manner as if the minimum device designation value (0: M device) is designated. Once designated, the setting is held until the device is designated again or until it is reset. A program error (P39) will occur if a device that does not exist is set.
(b) Device designation values
Device designa- tion value
Device Unit Device No.
Device designa- tion value
Device Unit Device No.
0 M Bit M0 to M10239 10 F Bit F0 to F1023 1 D Word D0 to D2047 13 L Bit L0 to L511 2 C Bit C0 to C255 18 V Bit V0 to V255 4 X * Bit X0 to X1FFF 19 ST Bit ST0 to ST63 5 Y * Bit Y0 to Y1FFF 20 SD Word SD0 to SD127 6 R Word R0 to R13311 21 SB* Bit SB0 to SB1FF 7 T Bit T0 to T703 22 SW* Word SW0 to SW1FF 9 SM Bit SM0 to SM127 23 B* Bit B0 to B1FFF 24 W* Word W0 to W1FFF
The unit is the amount of data per device No. «Word» has 16 bits, and «Bit» has one bit. * is a device that expresses the device No. as a hexadecimal.
13. Program Support Functions 13.5 User Macro Specifications
345
(2) Device No. designation (#100101)
The device to be read in is designated by substituting the device No. in this system variable. Convert a device expressed as a hexadecimal into a decimal when designating. If the data is read without designating this number, the data will be read in the same manner as if the minimum device No. (0) is designated. Once designated, the setting is held until the device No. is designated again or until it is reset. A program error (P39) will occur if a device No. that does not exist is set.
(3) Number of bytes designation (#100102)
(a) System variable for number of bytes designation The reading size is designated by substituting the number of bytes designation value in this system variable. If the data is read without designating this number, the data will be read in the same manner as if the minimum number of bytes designation value (0: bit designation) is designated. Once designated, the setting is held until the number of bytes is designated again or until it is reset. A program error (P39) will occur if a number of bytes that does not exist in the specifications is set.
(b) Number of bytes designation value
Read in data Operation Number of bytes
designa- tion value
Size Sign Range Word device Bit device
0 1 bit — 0 to 1 The number of bits designated is read in.
The bits for the designated device No. are read in.
1 1 byte No 0 to 255 101 Yes -128 to 127
The low-order byte is read in.
8 bits are read in from the designated device No.
2 2 bytes No 0 to 65535 102 Yes -32768 to 32767
Two bytes are read in.
16 bits are read in from the designated device No.
4 4 bytes No 0 to 4294967295 104 Yes -2147483648 to
2147483647
The designated device (L) and next device (H) are read in.
32 bits are read in from the designated device No.
0 to 4 are designated without a sign, and 101 to 104 are designated with a sign.
13. Program Support Functions 13.5 User Macro Specifications
346
(4) Bit designation (#100103)
(a) System variable for bit designation The bit to be read in is designated by substituting the bit designation value in this system variable. This designation is valid only when reading the bits for a 16-bit device, and is invalid in all other cases. If the data is read without designating this number, the data will be read in the same manner as if the minimum bit designation value (0: bit 0) is designated. Once designated, the setting is held until the bit is designated again or until it is reset. A program error (P39) will occur if a bit that does not exist is set.
(b) Bit designation values
Bit designation value Read in bit
0 Bit 0 1 Bit 1 : :
15 Bit 15
(5) PLC data read (#100110) The data for the designated device is read in with this system variable. Refer to the table for number of bytes designation for details on the range of data read in.
13. Program Support Functions 13.5 User Macro Specifications
347
Examples of programs for reading PLC data
(1) To read a bit device
#100100 = 0 ; …………Designates [M device]. #100101 = 0 ; …………Designates [Device No. 0]. #100102 = 0 ; …………Designates [Bit]. #100 = #100110 ; ……Reads M0 (one bit). #100102 = 1 ; …………Designates [1 byte]. #101 = #100110 ; ……Reads M0 to M7 (eight bits). (If M7 to M0 is 0001 0010, this will be #102 = 18 (0x12).) #100102 = 102 ; ……..Designates [Signed two bytes]. #102 = #100110 ; …..Reads M0 to M15 (16 bits). (If M15 to M0 is 1111 1110 1101 1100, this will be #102 = -292 (0xFEDC).) #100102 = 4 ; …………Designates [4 bytes]. #104 = #100110 ; …..Reads M0 to M31 (32 bits). (If M31 to M0 is 0001 0010 0011 0100 0101 0110 0111 1000, this will be #104 = 305419896 (0x12345678).)
(2) To read a word device #100100 = 1 ; …………Designates [D device]. #100101 = 0 ; …………Designates [Device No. 0]. #100102 = 0 ; …………Designates [Bit]. #100103 = 1 ; …………Designates [Bit 1]. #100 = #100110 ; ……Reads the D0 bit 1. (If D0 = 0x0102, this will be #101 =1.) #100102 = 1 ; …………Designates [1 byte]. #101 = #100110 ; …..Reads the low-order byte of D0. (If D0 = 0x0102, this will be #101 =2.) #100102 = 2 ; …………Designates [2 bytes]. #102 = #100110 ; …..Reads D0. (If D0 = 0x0102, this will be #102 =258.) #100102 = 104 ; ……..Designates [Signed four bytes]. #104 = #100110 ; …..Reads D0 and D1. (If D0 = 0xFFFE and D1 = 0xFFFF, this will be #104 =-2.)
13. Program Support Functions 13.5 User Macro Specifications
348
Examples of using macro program for reading PLC data
G340 F_. A_. Q_. H_. ; F_. ………..Number of bytes designation F0…… Designates bit. F1…… Designates one byte. F2…… Designates two bytes. A_. …………Device designation A0 ….. Designates M. A1 ….. Designates D. A2 ….. Designates C. A3 ….. Designates G. A4 ….. Designates X. A5 ….. Designates Y. A6 ….. Designates R. A7 ….. Designates T. Q_………….Device No. designation For a bit, designates the bit with two digits after the decimal point. For a byte, a decimal value is not designated. H_. ………… Storage common variable Designates the common variable No. for storing the read data.
#100100 = #1 ; ……. Designates device. #100101 = FIX [#17] ; ……. Designates device No. #100102 = #9 ; ……. Designates number of bytes. #100103 = FIX [#17100] MOD 100 ; ……. Designates bit. #[#11] = #100110 ; ……. Reads PLC data. M99 ;
Precautions for reading PLC data
(1) As the PLC data is read asynchronously from the ladder execution, the data is not necessarily
from the running program. Take care when reading devices that change.
(2) If reading of a device that does not exist is attempted by designating the device No. and number of bytes, the 0 value will be read in only for the sections that do not exist.
13. Program Support Functions 13.5 User Macro Specifications
349
Time reading variables
The following operations can be carried out using the system variable extension for the user macro time. (1) By adding time information system variable #3011 and #3012, the current date (#3011) and
current time (#3012) can be read and written.
(2) By adding parameter #1273/bit1, the unit (millisecond unit/hour unit) of the cumulative time during system variable #3002 automatic start can be changed.
Variable No. Details #3001 The cumulative time during power ON can be read and the value can be
substituted. The unit is a millisecond unit.
#3002 The cumulative time during automatic start can be read and the value can be substituted. The unit can be changed between millisecond and hour with parameter #1273/bit1.
#3011 The current date can be read and written. YYYY/MM/DD is read as a YYYYMMDD value. When a YYYYMMDD value is written in, it will be set as YY/MM/DD (the last two digits of the year are displayed). Command range for year/month/date setting Year (YYYY) : 2000 to 2099 Month (MM) : 1 to 12 Date (DD) : 1 to maximum number of days in month
#3012 The current time can be read and written. HH/MM/SS is read as a HHMMSS value. When an HHMMSS value is written in, it will be set as HH/MM/DD. Command range for hour/minute/second setting Hour (HH) : 0 to 23 (24-hour system) Minute (MM) : 0 to 59 Second (SS) : 0 to 59
(3) The cumulative time returns to 0 at approx. 2.44 1011 milliseconds (approx. 7.7 years).
(4) If a negative value or a value exceeding 244335917226 milliseconds (67871.08811851 hours for #3002 time designation) is set for the cumulative time, a program error (P35) will occur.
(5) If a value exceeding the command range is set for the date or time, a program error (P35) will occur.
(6) Always set the month/date/hour/minute/second as a two-digit value when setting the date and time.
If the value only has one digit, always add 0. (February 14, 2001 #3001= 20010214 ;, etc.)
13. Program Support Functions 13.5 User Macro Specifications
350
Examples of using time reading variable
(Example 1) To read the current date (February 14, 2001) in common variable #100 #100 = #3011 ; (20010214 is inserted in #100)
(Example 2) To write current time (18 hours, 13 minutes, 6 seconds) into system variable #3012 #3012 = 181306 ; (The command value cumulative time #2: time is set to 18:13:06.)
(Example 3) By setting the following type of program, the machining start/end time (year/month/date/hour/minute/second) can be viewed.
#100=#3011 ; Machining start year/month/date #101=#3012 ; Machining start hour/minute/second G28 X0 Y0 Z0 ; G92 ; G0 X50. ; . . . #102=#3011 ; Machining end year/month/date #103=#3012 ; Machining end hour/minute/second M30 ;
Restrictions and precautions for using time reading variable
(1) #3011 reads the date as an eight-digit value, so the difference of the two dates read in will not
be the difference of days.
(2) #3012 reads the time as a six-digit value, so the difference of the two times read in will not be the difference of hours.
13. Program Support Functions 13.5 User Macro Specifications
351
13.5.6 Arithmetic Commands
A variety of arithmetic operations can be performed between variables.
Command format
#i =
is a combination of constants, variables, functions and operators. Constants can be used instead of #j and #k below.
(1) Definition and substitution of variables #i = #j Definition, substitution
#i = #j + #k Addition #i = #j — #k Subtraction #i = #j OR #k Logical sum (at every bit of 32 bits)
(2) Addition arithmetic
#i = #j XOR #k Exclusive OR (at every bit of 32 bits) #i = #j #k Multiplication #i = #j / #k Division #i = #j MOD #k Remainder
(3) Multiplication arithmetic
#i = #j AND #k Logical product (at every bit of 32 bits) #i = SIN [#k] Sine #i = COS [#k] Cosine #i = TAN [#k] Tangent (sin/cos used for tan) #i = ASIN [#k] Arcsine #i = ATAN [#j] Arctangent (ATAN or ATN may be used) #i = ACOS [#j] Arc-cosine #i = SQRT [#k] Square root (SQRT or SQR may be used) #i = ABS [#k] Absolute value #i = BIN [#k] Conversion from BCD to BIN #i = BCD [#k] Conversion from BIN to BCD #i = ROUND [#k] Rounding off
(ROUND or RND may be used) #i = FIX [#k] Discard fractions less than 1 #i = FUP [#k] Add for fractions less than 1 #i = LN [#k] Natural logarithm
(4) Functions
#i = EXP [#k] Exponent with e (=2.718 …..) as bottom (Note 1) A value without a decimal point is basically treated as a value with a decimal point at the
end (1 = 1.000). (Note 2) Compensation amounts from #10001 and workpiece coordinate system offset values
from #5201 are handled as data with a decimal point. Consequently, data with a decimal point will be produced even when data without a decimal point have been defined in the variable numbers.
(Example)
#101 = 1000 ;
#10001 = #101 ;
#102 = #10001 ;
#101 1000.000 #102 1000.000
Common variables after execution
(Note 3) The after a function must be enclosed in the square parentheses.
13. Program Support Functions 13.5 User Macro Specifications
352
Sequence of arithmetic operations
(1) The sequence of the arithmetic operations (1) through (3) is, respectively, the functions
followed by the multiplication arithmetic followed in turn by the addition arithmetic.
#101 = #111 + #112SIN[#113] (1) Function
(2) Multiplication arithmetic
(3) Addition arithmetic
(2) The part to be given priority in the operation sequence should be enclosed in square
parentheses. Up to 5 pairs of such parentheses including those for the functions may be used. #101 = SQRT [ [ [ #111 = #112 ] SIN[#113] + #114] #15] ;
First pair of parentheses
Second pair of parentheses
Third pair of parentheses
Examples of arithmetic commands
(1) Main program and argument designation
G65 P100 A10 B20. ; #101=100.000 #102=200.000 ;
#1 #2 #101 #102
10.000 20.000
100.000 200.000
(2) Definition and substitution (=)
#1=1000 #2=1000. #3=#101 #4=#102 #5=#10001 (#10001=-10.)
#1 #2 #3 #4 #5
1000.000 1000.000
100.000 200.000 10.000
From common variables
From compensation amount
(3) Addition and subtraction (+, )
#11=#1+1000 #12=#250. #13=#101+#1 #14=#100013. (#10001 = -10.) #15=#10001+#102
#11 #12 #13 #14 #15
2000.000 950.000
1100.000 13.000 190.000
(4) Multiplication and division (, /)
#21=100100 #22=100.100 #23=100100 #24=100.100. #25=100/100 #26=100./100 #27=100/100. #28=100./100. #29=#10001#101
( #10001 = -10.) #30=#10001/#102
#21 #22 #23 #24 #25 #26 #27 #28 #29 #30
10000.000 10000.000 10000.000 10000.000
1.000 1.000 1.000 1.000
1000.000
-0.050
(5) Remainder (MOD)
#19=48 #20=9 #31=#19 MOD #20
#19/#20 = 48/9 = 5 with 3 over #31 = 3
13. Program Support Functions 13.5 User Macro Specifications
353
#3 = 01100100 (binary) 14 = 00001110 (binary)
(6) Logical sum (OR)
#3=100 #4=#3 OR 14
#4 = 01101110 = 110 #3 = 01100100 (binary) 14 = 00001110 (binary)
(7) Exclusive OR (XOR)
#3=100 #4=#3 XOR 14
#4 = 01101010 = 106 (8) Logical
product (AND)
#9=100 #10=#9 AND 15
#9 = 01100100 (binary) 15 = 00001111 (binary) #10 = 00000100 = 4
(9) Sin (SIN) #501 = SIN [60] #502 = SIN [60.] #503 = 1000SIN [60] #504 = 1000SIN [60.] #505 = 1000.SIN [60] #506 = 1000.SIN [60.] (Note) SIN [60] is equivalent to SIN [60.]
#501 #502 #503 #504 #505 #506
0.866 0.866
866.025 866.025 866.025 866.025
(10) Cosine (COS)
#541 = COS [45] #542 = COS [45.] #543 = 1000COS [45] #544 = 1000COS [45.] #545 = 1000.COS [45] #546 = 1000.COS [45.] (Note) COS [45] is equivalent to COS [45.]
#541 #542 #543 #544 #545 #546
0.707 0.707
707.107 707.107 707.107 707.107
(11) Tangent (TAN)
#551 = TAN [60] #552 = TAN [60.] #553 = 1000TAN [60] #554 = 1000TAN [60.] #555 = 1000.TAN [60] #556 = 1000.TAN [60.] (Note) TAN [60] is equivalent to TAN [60.]
#551 #552 #553 #554 #555 #556
1.732 1.732
1732.051 1732.051 1732.051 1732.051
#531 #432 #533 #534
30.000 30.000 30.000
-30.000
(12) Arcsine ASIN
#531 = ASIN [100.500/201.] #532 = ASIN [100.500/201] #533 = ASIN [0.500] #534 = ASIN [-0.500]
(Note) When #1273/bit 0 is set to 1, #534 will be 330.
(13) Arctangent (ATAN or ATN)
#561 = ATAN [173205/100000] #562 = ATAN [173205/100000.] #563 = ATAN [173.205/100] #564 = ATAN [173.205/100.] #565 = ATAN [1.73205]
#561 #562 #563 #564 #565
60.000 60.000 60.000 60.000 60.000
13. Program Support Functions 13.5 User Macro Specifications
354
(14) Arccosine
(ACOS) #521 = ACOS [100./141.421] #522 = ACOS [100./141.421]
#521 #522
45.000 45.000
(15) Square root (SQR or SQRT)
#571 = SQRT [1000] #572 = SQRT [1000.] #573 = SQRT [10. 10. +20. 20.] (Note) In order to increase the accuracy,
proceed with the operation inside parentheses.
#571 #572 #573
31.623 31.623 22.360
(16) Absolute value (ABS)
#576 = 1000 #577 = ABS [#576] #3 = 70. #4 = 50. #580 = ABS [#4 #3]
#576 #577 #580
1000.000 1000.000
120.000
(17) BIN, BCD #1 = 100 #11 = BIN [#1] #12 = BCD [#1]
#11 #12
64
256
(18) Rounding off (ROUND or RND)
#21 = ROUND [14/3] #22 = ROUND [14./3] #23 = ROUND [14/3.] #24 = ROUND [14./3.] #25 = ROUND [14/3] #26 = ROUND [14./3] #27 = ROUND [14/3.] #28 = ROUND [14./3.]
#21 #22 #23 #24 #25 #26 #27 #28
5 5 5 5
5 5 5 5
(19) Discarding fractions below decimal point (FIX)
#21 = FIX [14/3] #22 = FIX [14./3] #23 = FIX [14/3.] #24 = FIX [14./3.] #25 = FIX [14/3] #26 = FIX [14./3] #27 = FIX [14/3.] #28 = FIX [14./3.]
#21 #22 #23 #24 #25 #26 #27 #28
4.000 4.000 4.000 4.000
4.000 4.000 4.000 4.000
(20) Adding fractions less than 1 (FUP)
#21 = FUP [14/3] #22 = FUP [14./3] #23 = FUP [14/3.] #24 = FUP [14./3.] #25 = FUP [14/3] #26 = FUP [14./3] #27 = FUP [14/3.] #28 = FUP [14./3.]
#21 #22 #23 #24 #25 #26 #27 #28
5.000 5.000 5.000 5.000
5.000 5.000 5.000 5.000
(21) Natural logarithms (LN)
#101 = LN [5] #102 = LN [0.5] #103 = LN [5]
#101 #102 Error
1.609 0.693 «P282»
(22) Exponents (EXP)
#104 = EXP [2] #105 = EXP [1] #106 = EXP [2]
#104 #105 #106
7.389 2.718 0.135
13. Program Support Functions 13.5 User Macro Specifications
355
Arithmetic accuracy
As shown in the following table, errors will be generated when performing arithmetic operations once and these errors will accumulate by repeating the operations.
Arithmetic format Average error Maximum error Type of error a = b + c a = b c 2.33 1010 5.32 1010 Min. |/b|, |/c|
a = bc 1.55 1010 4.66 1010 a = b/c 4.66 1010 1.86 109 a = b 1.24 109 3.73 109
Relative error |/a|
a = SIN [b] a = COS [b] 5.0 109 1.0 108
a = ATAN [b/c] 1.8 106 3.6 106
Absolute error ||
(Note) SIN/COS is calculated for the function TAN.
Notes on reduced accuracy
(1) Addition and subtraction
It should be noted that when absolute values are used subtractively in addition or subtraction, the relative error cannot be kept below 108. For instance, it is assumed that the real values produced as the arithmetic calculation result of #10 and #20 are as follows (these values cannot be substituted directly) :
#10 = 2345678988888.888 #20 = 2345678901234.567
Performing #10 #20 will not produced #10 320 = 87654.321. There are 8 significant digits in the variables and so the values of #10 and #20 will be as follows (strictly speaking, the internal values will differ somewhat from the values below because they are binary numbers) :
#10 = 2345679000000.000 #20 = 2345678900000.000
Consequently, #10 #20 = 100000.000 will generate a large error.
(2) Logical operations EQ, NE, GT, LT, GE and LE are basically the same as addition and subtraction and so care should be taken with errors. For instance, to determine whether or not #10 and #20 are equal in the above example :
IF [#10EQ#20] It is not always possible to provide proper evaluation because of the above mentioned error. Therefore, when the error is evaluated as in the following expression :
IF [ABS [#10 #20] LT200000] and the difference between #10 and #20 falls within the designated range error, both values should be considered equal.
(3) Trigonometric functions
Absolute errors are guaranteed with trigonometric functions but since the relative error is not under 108, care should be taken when dividing or multiplying after having used a trigonometric function.
13. Program Support Functions 13.5 User Macro Specifications
356
13.5.7 Control Commands
The flow of programs can be controlled by IF-GOTO- and WHILE-DO-.
Branching
Format
IF [conditional expression] GOTO n; (n = sequence number in the program) When the condition is satisfied, control branches to «n» and when it is not satisfied, the next block is executed. IF [conditional expression] can be omitted and, when it is, control passes to «n» unconditionally. The following types of [conditional expressions] are available.
#i EQ #j = When #i and #j are equal #i NE #j When #i and #j are not equal #i GT #j > When #i is greater than #j #i LT #j < When #i is less than #j #i GE #j When #i is #j or more #i LE #j When #i is #j or less
«n» of GOTO n must always be in the same program. Program error (P231) will result if it is not. A formula or variable can be used instead of #i, #j and «n». In the block with sequence number «n» which will be executed after a GOTO n command, the sequence number must always be at the head of the block. Otherwise, program error (P231) will result. If «/» is at the head of the block and Nn follows, control can be branched to the sequence number.
Branching to N100 when content of #2 is 1
N10 #22=#20 #23=#21; IF [#2 EQ1] GOTO100; #22=#20-#3; #23=#21-#4; N100 X#22 Y#23; #1=#1+1;
B ra
nc h
se ar
ch
With N10
To head
Branch search
N100
(Note 1) When the sequence number of the branch destination is searched, the search is conducted up to the end of the program (% code) from the block following IF; and if it is not found, it is then conducted from the top of the program to the block before IF;. Therefore, branch searches in the opposite direction to the program flow will take longer to execute compared with branch searches in the forward direction.
(Note 2) EQ and NE should be used only for integers. For comparison of numeric values with
decimals, GE, GT, LE, and LT should be used.
13. Program Support Functions 13.5 User Macro Specifications
357
Iteration
Format
WHILE [conditional expression] DOm ; (m = 1, 2, 3 ….. 127) ~ END m ;
While the conditional expression is established, the blocks from the following block to ENDm are repeatedly executed; when it is not established, execution moves to the block after ENDm. DOm may come before WHILE, WHILE [conditional expression] DOm and ENDm must be used as a pair. IF WHILE [conditional expression] is omitted, these blocks will be repeatedly ad infinitum. The repeating identification numbers range from 1 through 127 (DO1, DO2, DO3, ……. DO127). Up to 27 nesting levels can be used.
(1) Same identifier number can be used any number of times.
Possible
Possible
WHILE ~ DO1 ; END1 ;
WHILE ~ DO1 ; END1 ;
(2) Any number may be used for the WHILE DOm identifier number.
Possible
WHILE ~ DO1 ; END1 ;
~
WHILE ~ DO3 ; END3 ;
~ ~
WHILE ~ DO2 ; END2 ;
~ ~
WHILE ~ DO1 ; END1 ;
~ ~
(3) Up to 27 nesting levels for WHILE DOm. «m» is
any number from 1 to 127 for the nesting depth.
Po ss
ib le
DO2
DO1
DO27
END 1 ;
WHILE ~ DO1 ;
WHILE ~ DO2 ;
WHILE~DO27;
END 2 ;
END 27 ;
:
:
(4) The number of WHILE DOm nesting levels cannot exceed 27.
N ot
p os
si bl
e WHILE ~ DO1 ;
WHILE ~ DO2 ;
WHILE ~ DO3 ;
WHILE ~ DO28;
END 3 ;
END 28;
~ ~
~ ~
END 2 ; :
END 1 ;
~
:
(Note) :With nesting, «m» which has been used once
cannot be used.
13. Program Support Functions 13.5 User Macro Specifications
358
(5) WHILE — DOm must be designated first and
ENDm last.
Not possible
END 1 ;
WHILE ~ DO1 ;
(6) WHILE — DOm and ENDm must correspond on a 1:1 (pairing) basis in the same program.
Not possible
END 1 ;
WHILE ~ DO1 ;
WHILE ~ DO1 ;
(7) Two WHILE — DOm’s must not overlap.
Not possible
END 2 ;
END 1 ;
WHILE ~ DO2 ;
WHILE ~ DO1 ;
~ ~
~
(8) Branching externally is possible from the WHILE — DOm range.
Possible
Nn
WHILE ~ DO1 ; IF ~ GOTOn ; END 1 ;
(9) No branching is possible inside WHILE — DOm.
N ot
p os
si bl
e
N ot
p os
si bl
e
END1;
IF~GOTOn;
END1;
IF~GOTOn;
Nn;
END1;
WHILE~DO1;
WHILE~DO1;
Nn;
WHILE~DO1;
(10) Subprograms can be called by M98, G65 or G66 between WHILE — DOm’s.
Po ss
ib le
G65 P100; END1;
Main program
WHILE~DO1; WHILE~DO02;
END2;
M99;
Subprogram
M02;
To subprogram
(11) Calls can be initiated by G65 or G66 between WHILE — DOm’s and commands can be issued again from 1. Up to 27 nesting levels are possible for the main program and subprograms.
WHILE ~ DO1 ; END 1 ; M99 ;
WHILE ~ DO1 ; G65 P100 ; END 1 ;
Subprogram Main program
Po ss
ib le
To subprogram
M02 ;
~ ~
~
(12) A program error will occur at M99 if WHILE and END are not paired in the subprogram (including macro subprogram).
Don ENDn constitutes illegal usage.
WHILE
~DO1;
M99;
Main program Subprogram M98 P100;
M02;
To subprogram
(Note) As the canned cycles G73 and G83 and the special canned cycle G34 use WHILE, these will be added multiple times.
13. Program Support Functions 13.5 User Macro Specifications
359
13.5.8 External Output Commands Function and purpose
Besides the standard user macro commands, the following macro instructions are also available as external output commands. They are designed to output the variable values or characters via the RS-232C interface.
Command format
POPEN For preparing the processing of data outputs PCLOS For terminating the processing of data outputs BPRNT For character output and variable value binary output DPRNT For character output and digit-by-digit variable numerical output
Command sequence
POPEN
DPRNT
PCLOS
Open command
Data output command
Closed command
Open command : POPEN
(1) The command is issued before the series of data output commands. (2) The DC2 control code and % code are output from the NC system to the external output
device. (3) Once POPEN; has been issued, it will remain valid until PCLOS; is issued.
Close command : PCLOS
(1) This command is issued when all the data outputs are completed. (2) The DC4 control code and % code are output from the NC unit to the external output device. (3) This command is used together with the open command and it should not be issued unless the
open mode has been established. (4) Issue the close command at the end of the program even when operation has been
suspended by resetting or some other operation during data output.
13. Program Support Functions 13.5 User Macro Specifications
360
Data output command : DPRNT
DPRNT [ l1 # v1 [ d1 c1 ] l 2 # v2 [ d2 c2 ] ] l1 : Character string v1 : Variable number d1 : Significant digits above decimal point c1 : Significant digits below decimal point
(1) The character output and decimal output of the variable values are done with ISO codes. (2) The commanded character string is output as is by the ISO code. Alphanumerics (A to Z, 0 to 9) and special characters (+, , , /) can be used.
Note that asterisk (*) is output as a space code. (3) The required significant digits above and below the decimal point in the variable values are
commanded within square parentheses. As a result, the variable values equivalent to the commanded number of digits including the decimal point are output in ISO code in decimal notation from the high-order digits. Trailing zeroes are not omitted.
(4) Leading zeroes are suppressed. The leading zeroes can also be replaced by blank if so specified with a parameter. This can
justify printed data on the last column.
(Note) A data output command can be issued even in two-part system mode. In this case, however, note that the output channel is shared for both part systems. So, take care not to execute data output in both part systems simultaneously.
c + d 8
13. Program Support Functions 13.5 User Macro Specifications
361
13.5.9 Precautions Precautions
When the user macro commands are employed, it is possible to use the M, S, T and other NC control commands together with the arithmetic, decision, branching and other macro commands for preparing the machining programs. When the former commands are made into executable statements and the latter commands into macro statements, the macro statement processing should be accomplished as quickly as possible in order to minimize the machining time, because such processing is not directly related to machine control. As a result, the parameter «#8101 macro single» can be set and the macro statements can be processed in parallel with the execution of the executable statement. (The parameter can be set OFF during normal machining to process all the macro statements together or set ON during a program check to execute the macro statements block by block. This enables the setting to be made in accordance with the intended objective in mind.)
G91G28X0Y0Z0 ; (1) G92X0Y0Z0 ; (2) G00X-100.Y-100. ; (3) #101=100. COS [210.] ; (4) #102=100. SIN [210.] ; (5)
G01X#101Y#102F800 ; (6)
Example of program
Macro statement
Macro statements are: (1) Arithmetic commands (block including =) (2) Control commands (block including GOTO, DO-END, etc.) (3) Macro call commands (including macro calls based on G codes and cancel commands (G65,
G66, G66.1, G67)) Executable statements indicate statements other than macro statements.
Flow of processing
M ac
ro s
in gl
e O
FF
(1) (2) (4)(5)(6)(3)
(1) (2) (4)(5)(6) (3)
Program analysis
Block executing
M ac
ro s
in gl
e O
N
Program analysis
Block executing
(1) (2) (3)
(1) (2) (3)
(4) (5) (6)
(4) (5) (6)
13. Program Support Functions 13.5 User Macro Specifications
362
Machining program display
M ac
ro s
in gl
e O
N
[In execution] N3 G00 X-100. Y-100. ; [Next command]N6 G01 X#101 Y#102
F800 ;
N4, N5 and N6 are processed in parallel with the control of the executable statement of N3, N6 is an executable statement and so it is displayed as the next command. If the N4, N5 and N6 analysis is in time during N3 control, the machine movement will be continuously controlled.
M ac
ro s
in gl
e O
FF
[In execution]
N3 G00 X-100. Y-100. ; [Next command]
N4 #101=100. COS [210.] ;
N4 is processed in parallel with the control of the NC executable statement of N3, and it is displayed as the next command. N5 and N6 is executed after N3 has finished, and so the machine control is held on standby during the N5 and N6 analysis time.
13. Program Support Functions 13.5 User Macro Specifications
363
13.5.10 Actual Examples of Using User Macros
The following three examples will be described. (Example 1) SIN curve (Example 2) Bolt hole circle (Example 3) Grid
(Example 1) SIN curve
G65 Pp1 Aa1 Bb1 Cc1 Ff1 ;
a1 ; Initial value 0 b1 ; Final value 360 c1 ; R of %SIN f1 ; Feedrate
(SIN) Y
X
100.
-100.
0 90. 270. 360.180.
Local variable set by argument
To subprogram
(Note 1) Commanding with one block is possible when G90G01X#1Y [#3SIN [#1]] F#9 ; is issued.
G65P9910A0B360.C100.F100;
#1=0 #2=360.000 #3=100.000 #9=100.000
WHILE [#1LE#2] DO1; #101=#3SIN [#1] ; G90G01X#1Y#10F#9; #1=#1+10.; END1; M99;
~ ~
Main program O9910 (Subprogram)
(Note 1)
13. Program Support Functions 13.5 User Macro Specifications
364
(Example 2) Bolt hole circle
After defining the hole data with canned cycle (G72 to G89), the macro command is issued as the hole position command.
G81Z100.R50.F300L0 G65P9920Aa1Bb1Rr1Xx1Yy1 ;
-Y
y1
W x1 -X
a1
#101=0 ; #102=#4003 ; #103=#5001 ; #104=#5002 ; #111=#1 ; WHILE [#101LT#2] DO1 ; #120=#24+#18COS [#111] ; #121=#25+#18SIN [#111] ; #122=#120 #123=#121 ; IF [#102EQ90] GOTO100 ; #122=#120 #103 ; #123=#121 #104 ; #103=#120 #104=#121 N100 X#122Y#123 ; #101=#101+1 ; #111=#1+360.#101/#2 ; END1 ; M99 ;
Main program
O9920 (Subprogram)
(Note 1) The processing time can be shortened by programming in one block.
a1 ; Start angle b1 ; No. of holes r1 ; Radius x1 ; X axis center position y1 ; Y axis center position
(Note 1)
(Note 1)
(Note 1)
To subprogram
O9920
0 #101 G90, G91 mode Read in #102 Read previous coordinates
X #103 Y #104 Start angle 111
#101 = No. of hole count #102 = G90 or G91 #103 = X axis current position #104 = Y axis current position #111 = Start angle
#101 No. of holes
#102=90
RadiusCOS [#111] + Center coordinates X#120 RadiusSIN [#111] + Center coordinates Y#121 #120 #122 #121 #123
#120 = Hole position X coordinates #121 = Hole position Y coordinates #122 = X axis absolute value #123 = Y axis absolute value
END
#120-#103 #122 #121-#104 #123 #120 #103 #121 #104
#122 = X axis incremental value 123 = Y axis incremental value X axis current position update Y axis current position update
Judgment of G90, G91 mode
#101+1 #101 360 deg.#101/ No. of holes+#1 #111
No.of holes counter up #111 = Hole position angle
N100X#122Y#123 Drilling command
Y
N
N
Y
(Note 1)
(Note 1)
13. Program Support Functions 13.5 User Macro Specifications
365
To subprogram
To subprogram
To subprogram
-Y
-500.
W -500.-X
300R
100R
200R
G28 X0 Y0 Z0; T1 M06; G90 G43 Z100.H01; G54 G00 X0 Y0; G81 Z-100.R3.F100 L0 M03; G65 P9920 X-500. Y-500. A0 B8 R100.; G65 P9920 X-500. Y-500. A0 B8 R200.; G65 P9920 X-500. Y-500. A0 B8 R300.;
(Example 3) Grid After defining the hole data with the canned cycle (G72 to G89), macro call is commanded as a hole position command.
Subprogram is on next page
-Y
y1
W x1 -X
i1 G81 Zz1 Rr1 Ff1; G65Pp1 Xx1 Yy1 Ii1 Jj1 Aa1 Bb1;
j1
x1 ; X axis hole position y1 ; Y axis hole position i1 ; X axis interval j1 ; Y axis interval a1 ; No. of holes in X direction b1 ; No. of holes in Y direction
To subprogram
To subprogram
-Y
W
-X
-X
-Z
G28 X0 Y0 Z0; T1 M06; G90 G43 Z100.H01; G54 G00 X0 Y0; G81 Z-100. R3.F100 L0 M03; G65 P9930 X0 Y0 I-100. J-75. A5B3; G84 Z-90. R3. F250 M03; G65 P9930 X0 I-100. J-75. A5B3;
-75.
-75.
-100.
100. 100. 100.
13. Program Support Functions 13.5 User Macro Specifications
366
O9930 (Subprogram) O9930
#101=#24 ;
#102=#25 ;
#103=#4 ;
#104=#5 ;
#106=#2 ;
WHILE [#106GT0] DO1 ;
#105=#1 ;
WHILE [#105GT0] DO2 ;
G90 X#101 Y#102 ;
#101=#101+#103 ;
#105=#1051 ;
END2 ;
#101=#101-#103;
#102=#102+#104;
#103=#103 ;
#106=#1061 ;
END1 ;
M99 ;
(Note 1) The processing time can be shortened by programming in one block.
(Note 1)
(Note 1)
(Note 1)
Start point X coordinates : x1#101 Start point Y coordinates : y1#102 X axis interval : i1#103 Y axis interval : j1#104 No. of holes in Y direction : b1#106
#101 = X axis start point #102 = Y direction interval #103 = X direction interval #106 = No. of holes in Y direction
#106 > 0
Y direction drilling completion check
#105 > 0
X#101 Y#102
#101 + #103 #101
#105 1 #105
#101 #103 #101 #102 + #104 #102
#103 #103
#106 1 #106
END N
Y
No. of holes in Y direction No. of holes in X direction set No. of holes in Y direction check Positioning, drilling X coordinates update No. of holes in X direction 1 X coordinates revision Y coordinates update X axis drilling direction reversal No. of holes in Y direction 1
13. Program Support Functions 13.6 G Command Mirror Image; G50.1, G51.1
367
13.6 G Command Mirror Image; G50.1, G51.1
Function and purpose
When cutting a shape that is symmetrical on the left and right, programming time can be shortened by machining the one side and then using the same program to machine the other side. The mirror image function is effective for this. For example, when using a program as shown below to machine the shape on the left side, a symmetrical shape can be machined on the right side by applying mirror image and executing the program.
Base shape (program) Shape when machining program
for left side is executed after the mirror command.
Mirror axis
Y
X
Command format
G51.1 Xx1 Yy1 Zz1 ; Mirror image ON G50.1 Xx2 Yy2 Zz2 ; Mirror image OFF x1, y1, z1: Mirror image center coordinates
(Mirror image will be applied regarding this position as a center) x2, y2, z2: Mirror image cancel axis
(The values of x2, y2, z2 will be ignored.) Command these items with the absolute or incremental position.
Detailed description
(1) At G51.1, command the mirror image axis and the coordinate to be a center of mirror image
with the absolute command or incremental command. (2) At G50.1, command the axis for which mirror image is to be turned OFF.
The values of x2, y2, and z2 will be ignored. (3) If mirror image is applied on only one axis in the designated plane, the rotation direction and
compensation direction will be reversed for the arc or tool radius compensation and coordinate rotation, etc.
(4) This function is processed on the local coordinate system, so the center of the mirror image
will change when the counter is preset or when the workpiece coordinates are changed.
13. Program Support Functions 13.6 G Command Mirror Image; G50.1, G51.1
368
(5) Reference position return during mirror image
If the reference position return command (G28, G30) is executed during the mirror image, the mirror image will be valid during the movement to the intermediate point, but will not be applied on the movement to the reference position after the intermediate point.
Intermediate point when mirror is applied
Path on which mirror is applied
Intermediate point
Programmed path
Mirror center
(6) Return from zero point during mirror image
If the return command (G29) from the zero point is commanded during the mirror image, the mirror will be applied on the intermediate point.
(7) The mirror image will not be applied on the G53 command.
13. Program Support Functions 13.6 G Command Mirror Image; G50.1, G51.1
369
Precautions
CAUTION
Turn the mirror image ON and OFF at the mirror image center.
If mirror image is canceled at a point other than the mirror center, the absolute value and machine position will deviate as shown below. (In this state, execute the absolute value command (positioning with G90 mode), or execute reference position return with G28 or G30 to continue the operation.) The mirror center is set with an absolute value, so if the mirror center is commanded again in this state, the center may be set to an unpredictable position. Cancel the mirror at the mirror center or position with the absolute value command after canceling.
Absolute value (position commanded in program) Machine position
When moved with the incremental command after mirror cancel
Issue mirror cancel command here
Issue mirror axis command here Mirror center
Combination with other functions
(1) Combination with radius compensation
The mirror image (G51.1) will be processed after the radius compensation (G41, G42) is applied, so the following type of cutting will take place.
Programmed path
When only radius compensation is applied
Mirror center
When only mirror image is applied
When both mirror image and radius compensation are applied
13. Program Support Functions 13.7 Corner Chamfering/Corner Rounding I
370
13.7 Corner Chamfering/Corner Rounding I
Chamfering at any angle or corner rounding is performed automatically by adding «,C_» or «,R_» to the end of the block to be commanded first among those command blocks which shape the corner with lines only.
13.7.1 Corner Chamfering » ,C_ »
Function and purpose
The corner is chamfered in such a way that the positions produced by subtracting the lengths commanded by «,C_» from the imaginary starting and final corners which would apply if no chamfering were to be performed, are connected.
Command format
N100 G01 X__ Y__ ,C__ ; N200 G01 X__ Y__ ; ,C : Length up to chamfering starting point or end point from imaginary corner
Chamfering is performed at the point where N100 and N200 intersect.
Example of program
(1) G91 G01 X100., C10. ; (2) X100. Y100. ;
Imaginary corner intersection point
Chamfering start point
Chamfering end point
Y axis
X axis
X100.0 X100.0
10.0
10.0
Y100.0
(1)
(2)
13. Program Support Functions 13.7 Corner Chamfering/Corner Rounding I
371
Detailed description
(1) The start point of the block following the corner chamfering serves as the imaginary corner
intersection point. (2) When the comma in «,C» is not present, it is handled as a C command. (3) When both the corner chamfer and corner rounding commands exist in the same block, the
latter command is valid. (4) Tool compensation is calculated for the shape which has already been subjected to corner
chamfering. (5) When scaling is commanded, scaling will also be applied to the commanded corner chamfer
amount. (6) Program error (P381) results when there is an arc command in the block following the corner
chamfering block. (7) Program error (P382) results when the block following the corner chamfering block does not
have a linear command. (8) Program error (P383) results when the movement amount in the corner chamfering block is
less than the chamfering amount. (9) Program error (P384) results when the movement amount in the block following the corner
chamfering block is less than the chamfering amount.
13. Program Support Functions 13.7 Corner Chamfering/Corner Rounding I
372
13.7.2 Corner Rounding » ,R_ »
Function and purpose
The imaginary corner, which would exist if the corner were not to be rounded, is rounded with the arc having the radius which is commanded by «,R_» only when configured of linear lines.
Command format
N100 G01 X__ Y__ , R__ ; N200 G02 X__ Y__ ; ,R : Arc radius of corner rounding
Corner rounding is performed at the point where N100 and N200 intersect. Example of program
(1) G91 G01 X100., R10. ; (2) X100. Y100. ;
Y axis
Corner rounding end point
Corner rounding start point
Imaginary corner intersection point
X axis
X100.0 X100.0
Y100.0
(1)
(2)
R10.0
Detailed description
(1) The start point of the block following the corner R serves as the imaginary corner intersection
point. (2) When the comma in «,R» is not present, it is handled as an R command. (3) When both the corner chamfer and corner rounding commands exist in the same block, the
latter command is valid. (4) Tool compensation is calculated for the shape which has already been subjected to corner
rounding. (5) Program error (P381) results when there is an arc command in the block following the corner
rounding block. (6) Program error (P382) results when the block following the corner rounding block does not
have a linear command. (7) Program error (P383) results when the movement amount in the corner rounding block is less
than the R value. (8) Program error (P384) results when the movement amount in the block following the corner
rounding block is less than the R value.
13. Program Support Functions 13.8 Linear Angle Command
373
13.8 Linear Angle Command
Function and purpose
The end point coordinates are calculated automatically by commanding the linear angle and one of the end point coordinate axes.
Command format
N1 G01 Xx1 (Yy1) Aa1; N1 G01 Xx2 (Yy 2) Aa2; (A-a2 can also be set as As3.) or N1 G01 Xx1 (Yy 1) ,Aa1; N1 G01 Xx2 (Yy 2) ,Aa2;
This designates the angle and the X or Y axis coordinates. Select the command plane with G17 to G19.
Y
y2
y1 (x1,y1)
N1
X
N2
a1
a2
a3
(x2,y2)
Detailed description
(1) The angle is from the + direction of the horizontal axis on the selected plane. The counter-
clockwise (CCW) direction is considered to be + and the clockwise direction (CW) .
(2) Either of the axes on the selected plane is commanded for the end point.
(3) The angle is ignored when the angle and the coordinates of both axes are commanded.
(4) When only the angle has been commanded, this is treated as a geometric command.
(5) The angle of either the start point (a1) or end point (a2) may be used.
(6) This function is valid only for the G01 command; it is not valid for other interpolation or positioning commands.
(7) The range of slope «a» is 360.000 a 360.000. When a value outside this range is commanded, it will be divided by 360 (degrees) and the
remainder will be commanded. (Example) If 400 is commanded, 40 (remainder of 400/360) will become the command angle.
(8) If address A is used for the axis name or 2nd miscellaneous function, use «,A» as the angle.
(9) If «A» and «,A» are commanded in the same block, «,A» will be interpreted as the angle.
(Note) A program error (P33) will occur if this function is commanded during the high-speed
machining mode or high-speed high-accuracy mode.
13. Program Support Functions 13.9 Geometric Command
374
13.9 Geometric Command
Function and purpose
When it is difficult to find the intersection point of two straight lines with a continuous linear interpolation command, this point can be calculated automatically by programming the command for the angle of the straight lines. Example
N 1
a 2
X
Z W 1
N 2
a1
N1 G01 Aa1 Ff1 ; N2 Xx1 Zz1 Aa2 ;
End point (X1, Z1)
Automatic intersection point calculation
Z1
x1 2
Start point
a: Angle () formed between straight line and horizontal axis on plane. The plane is the selected plane at this time.
(Note 1) This function cannot be used when using the A axis or 2nd miscellaneous function A.
Command format
N1 G01 Xx1 (Yy1) Aa1; N1 G01 Xx2 (Yy 2) Aa2; (A-a2 can also be set as As3.)
This designates the angle and the X or Y axis coordinates. Select the command plane with G17 to G19.
13. Program Support Functions 13.9 Geometric Command
375
Detailed description
(1) Automatic calculation of two-arc contact
When two continuous circular arcs contact with each other and it is difficult to find the contact, the contact is automatically calculated by specifying the center coordinates position or radius of the first circular arc and the end point (absolute position) and center position or radius of the second circular arc. Example
G18 G02 Ii1 Kk1 Ff1 ; G03 Xxc Zzc Ii2 Kk2 Ff2 ;
OR G18 G02 Ii1 Kk1 Ff1 ; G03 Xxc Zzc Rr2 Ff2 ;
OR G18 G02 Rr1 Ff1 ;
G03 Xxc Zzc Ii2 Kk2 Ff2 ;
C(xc, zc)
r2
(p2,q2)
(p1,q1)
B(?,?) r1
A
I and K : Incremental position from arc end point P and Q : Arc center position (absolute position)
I and K are the arc center position (incremental position); distances from the start point in the first block or distances from the end point in the second block. P and Q (X, Z arc center position (absolute position)) can be commanded instead of I and K commands.
13. Program Support Functions 13.9 Geometric Command
376
(2) Automatic calculation of linear-arc intersection
When it is difficult to find the intersections of a given line and circular arc, the intersections are automatically calculated by programming the following blocks. Example
G18 G01 Aa1 Ff1 ;
G02 Xxc Zzc Ii2 Kk2 Hh2 Ff2 ;
r1
(p2,q2)
B(?,?)
B(?,?) a1
A C(xc, zc)
I and K : Incremental position from arc end point P and Q : Arc center position (absolute position) H = 0 : Intersection with shorter line (B point) H = 1 : Intersection with longer line (B point)
(3) Automatic calculation of arc-linear intersection
When it is difficult to find the intersections of a given circular arc and line, the intersections are automatically calculated by programming the following blocks. Example
G18 G03 Ii1 Kk1 Hh1 Ff1 ;
G01 Xxc Zzc Aa1 Ff1 ;
r1
a1
C(xc, zc)
B(?,?) B(?,?) (p1,q1)
A
I and K : Incremental position from arc end point P and Q : Arc center position (absolute position) (L3 only) H = 0 : Intersection with shorter line (B point) H = 1 : Intersection with longer line (B point)
13. Program Support Functions 13.9 Geometric Command
377
(4) Automatic calculation of linear-arc contact
When it is difficult to find the contact of a given line and circular arc, the contact is automatically calculated by programming the following blocks.
Example G01 Aa1 Ff1 ; G03 Xxc Zzc Rr1 Ff1 ;
a1
A
B (?,?)
r1
C(xc, zc)
(5) Automatic calculation of arc-linear contact
When it is difficult to find the contact of a given circular arc and line, the contact is automatically calculated by programming the following blocks.
Example G02 Rr1 Ff1 ; G01 Xxc Zzc Aa1 Ff1 ;
a1 r1
A B (?,?)
C(xc, zc)
13. Program Support Functions 13.10 Circle Cutting; G12, G13
378
13.10 Circle Cutting; G12, G13
Function and purpose
Circle cutting starts the tool from the center of the circle, and cuts the inner circumference of the circle. The tool continues cutting while drawing a circle and returns to the center position.
Command format
G12 (G13) I__ D__ F__ ; G12 : Clockwise (CW) G13 : Counterclockwise (CCW) I : Radius of circle (incremental value), the symbol is ignored D : Offset No. (The offset No. and offset data are not displayed on the setting
and display unit.) F : Feedrate
Detailed description
(1) The symbol + for the offset amount indicates reduction, and indicates enlargement. (2) The circle cutting is executed on the plane G17, G18 or G19 currently selected.
d1 offset amount +
d1 offset amount
Offset amount symbol + Offset amount symbol
For G12 (tool center path) 0 1 2 3 4 5 6 7 0
For G13 (tool center path) 0 7 6 5 4 3 2 1 0
5
2 1
7 64
3
i1
X
Y
0
Circle radius
13. Program Support Functions 13.10 Circle Cutting; G12, G13
379
Example of program
(Example 1) G12 I5000 D01 F100 ; (Input setting unit 0.01)
When compensation amount is +10.00mm
Tool
Compensation amount
Radius
X
Y
50.000m
10.000m
Precautions
(1) If the offset No. «D» is not issued or if the offset No. is illegal, the program error (P170) will
occur. (2) If [Radius (I) = offset amount] is 0 or negative, the program error (P233) will occur. (3) If G12 or G13 is commanded during radius compensation (G41, G42), the radius
compensation will be validated on the path after compensating with the D commanded with G12 or G13.
(4) If an address, not included in the format, is commanded in the same block as G12 and G13, a program error (P32) will occur.
13. Program Support Functions 13.11 Parameter Input by Program ; G10, G11
380
13.11 Parameter Input by Program; G10, G11
Function and purpose
The parameters set from the setting and display unit can be changed in the machining programs. The range of command data depends on the parameter setting range described in the Setup Manual. The data format used for the data setting is as follows.
Command format
G10 L70 ; Data setting start command P parameter No. S part system No. A axis No. H data ; . . . . . . . . . . . P parameter No. S part system No. A axis No. D data ; . . . . . . . . . . . . P parameter No. S part system No. A axis No. . . .
Bit parameter Numerical value parameter Character string parameter
G11 Data setting end command
(Note 1) The sequence of addresses in a block must be as shown above. When an address is commanded two or more times, the last command will be valid.
(Note 2) The part system No. is set in the following manner: «1» for 1st part system, «2» for 2nd part system, and so forth. If the address S is omitted, the part system of the executing program will be applied As for the parameters common to part systems, the command of part system No. will be ignored.
(Note 3) The axis No. is set in the following manner: «1» for 1st axis, «2» for 2nd axis, and so forth. If the address A is omitted, the 1st axis will be applied. As for the parameters common to axes, the command of axis No. will be ignored.
(Note 4) Address H is commanded with the combination of setting data (0 or 1) and the bit designation ( ) (0 to 7).
(Note 5) Only the decimal number can be commanded with the address D. The value that is smaller than the input setting increment (#1003 iunit) will be round off to the nearest increment.
(Note 6) The character string must be put in angled brackets «<» and «>». If these brackets are not provided, the program error (P33) will occur. Up to 63 characters can be set.
(Note 7) Command G10L70, G11 in independent blocks. A program error (P33, P421) will occur if not commanded in independent blocks.
Example of program
(Example)
G10 L70; P6401 H71 ; Sets 1 to #6401 bit7. P8204 S1 A2 D1.234 ; Sets 1.234 to #8204 of the 1st part system 2nd axis. P8621 ; Sets x to #8621. G11
13. Program Support Functions 13.12 Macro Interrupt ; M96, M97
381
13.12 Macro Interrupt; M96, M97
Function and purpose
A user macro interrupt signal (UIT) is input from the machine to interrupt the program being currently executed and instead call another program and execute it. This is called the user macro interrupt function. Use of this function allows the program to operate flexibly enough to meet varying conditions. For setting the parameters of the function, refer to the Setup manual.
Command format
M96 P__ H__ ; or M96 <File name> H__ ;
User macro interruption enable
M96 P H
:User macro interruption command :Interrupt program No. :File name A file name can be specified instead of a program No. In this case, enclose the file name with brackets <>. (The file name can have up to 32 characters including the extension.) :Interrupt sequence No.
M97 ; User macro interruption disable M97 :User macro interruption end command
The user macro interrupt function is enabled and disabled by the M96 and M97 commands programmed to make the user macro interrupt signal (UIT) valid or invalid. That is, if an interrupt signal (UIT) is input from the machine side in a user macro interrupt enable period from when M96 is issued to when M97 is issued or the NC is reset, a user macro interrupt is caused to execute the program specified by P__ instead of the one being executed currently. Another interrupt signal (UIT) is ignored while one user macro interrupt is being in service. It is also ignored in a user macro interrupt disable state such as after an M97 command is issued or the system is reset. M96 and M97 are processed internally as user macro interrupt control M codes.
Interrupt enable conditions
A user macro interrupt is enabled only during execution of a program. The requirements for the user macro interrupt are as follows: (1) An automatic operation mode or MDI has been selected. (2) The system is running in automatic mode. (3) No other macro interrupt is being processed.
(Note 1) A macro interrupt is disabled in manual operation mode (JOG, STEP, HANDLE, etc.)
13. Program Support Functions 13.12 Macro Interrupt ; M96, M97
382
Outline of operation
(1) When a user macro interrupt signal (UIT) is input after an M96Pp1 ; command is issued by the
current program, interrupt program Op1 is executed. When an M99; command is issued by the interrupt program, control returns to the main program.
(2) If M99Pp2 ; is specified, the blocks from the one next to the interrupted block to the last one are searched for the block with sequence number Np2 ;. Control thus returns to the block with sequence number Np2 that is found first in the above search. Current program
User macro interrupt signal (UIT)
Interrupt program
M96Pp1;
Np2 ;
M97 ;
Op1 ;
M99(Pp2) ;
Interrupt signal (UIT) not acceptable within a user macro program
(If Pp2 is specified)
Np2 ;
«User macro interruption»
signal is acceptable.
«User macro interruption»
signal is not acceptable. M30 ;
13. Program Support Functions 13.12 Macro Interrupt ; M96, M97
383
Interrupt type
Interrupt types 1 and 2 can be selected by the parameter «#1113 INT_2».
[Type 1] When an interrupt signal (UIT) is input, the system immediately stops moving the tool and
interrupts dwell, then permits the interrupt program to run. If the interrupt program contains a move or miscellaneous function (MSTB) command, the
commands in the interrupted block are lost. After the interrupt program completes, the main program resumes operation from the block next to the interrupted one.
If the interrupt program contains no move and miscellaneous (MSTB) commands, it resumes operation, after completion of the interrupt program, from the point in the block where the interrupt was caused.
If an interrupt signal (UIT) is input during execution of a miscellaneous function (MSTB) command, the NC system waits for a completion signal (FIN). The system thus executes a move or miscellaneous function command (MSTB) in the interrupt program only after input of FIN.
[Type 2] When an interrupt signal (UIT) is input, the interrupt program will be executed in parallel with the
executing block. If the interrupt program contains a move or miscellaneous function (MSTB) command, the
commands in the interrupted block are completed, then, these commands will be executed. If the interrupt program contains no move and miscellaneous function (MSTB) commands, the
interrupt program is executed without interrupting execution of the current block.
However, if the interrupt program has not ended even after the execution of the original block is completed, the system may stop machining temporarily.
13. Program Support Functions 13.12 Macro Interrupt ; M96, M97
384
[Type 1]
Interrupt program
If the interrupt program contains a move or miscellaneous function command, the reset block (2) is lost.
If the interrupted program contains no move and miscellaneous commands, it resumes operation from where it left in block (2), that is, all the reset commands.
block(2)
block(2) block(2)
block(2) Main program
block(1) block(3)
block(1) block(3)
block(1) block(3)
User macro interrupt
Interrupt program
User macro interrupt
Executing
[Type 2]
block(2)
block(2)
block(2) Main program
block(1) block(3)
block(1) block(3)
block(1) block(3)
If the interrupted program contains no move and miscellaneous commands, the interrupted program is kept executed in parallel to execution of the interrupt program block (3).
The move or miscellaneous command in the interrupt program is executed after completion of the current block.
Interrupt program
User macro interrupt signal
Interrupt program
User macro interrupt
13. Program Support Functions 13.12 Macro Interrupt ; M96, M97
385
Calling method
User macro interrupt is classified into the following two types depending on the way an interrupt program is called. These two types of interrupt are selected by parameter «#1229 set01/bit0». Both types of interrupt are included in calculation of the nest level. The subprograms and user macros called in the interrupt program are also included in calculation of the nest level. a. Subprogram type interrupt b. Macro type interrupt
Subprogram type interrupt The user macro interrupt program is called as a subprogram. As with calling by M98, the local variable level remains unchanged before and after an interrupt.
Macro type interrupt The user macro interrupt program is called as a user macro. As with calling by G65, the local variable level changes before and after an interrupt. No arguments in the main program can be passed to the interrupt program.
Acceptance of user macro interrupt signal (UIT)
A user macro interrupt signal (UIT) is accepted in the following two modes: These two modes are selected by a parameter «#1112 S_TRG». a. Status trigger mode b. Edge trigger mode
Status trigger mode The user macro interrupt signal (UIT) is accepted as valid when it is on. If the interrupt signal (UIT) is ON when the user macro interrupt function is enabled by M96, the interrupt program is activated. By keeping the interrupt signal (UIT) ON, the interrupt program can be executed repeatedly.
Edge trigger mode The user macro interrupt signal (UIT) is accepted as valid at its rising edge, that is, at the instance it turns on. This mode is useful to execute an interrupt program once.
User macro interrupt signal (UIT)
(Status trigger mode)
(Edge trigger mode)
User macro interrupt
ON
OFF
Accepting user macro interrupt signal (UIT)
13. Program Support Functions 13.12 Macro Interrupt ; M96, M97
386
Returning from user macro interrupt
M99 (P__) ; An M99 command is issued in the interrupt program to return to the main program. Address P is used to specify the sequence number of the return destination in the main program. The blocks from the one next to the interrupted block to the last one in the main program are first searched for the block with designated sequence number. If it is not found, all the blocks before the interrupted one are then searched. Control thus returns to the block with sequence number that is found first in the above search. (This is equivalent to M99P__ used after M98 calling.)
Modal information affected by user macro interrupt
If modal information is changed by the interrupt program, it is handled as follows after control returns from the interrupt program to the main program. Returning with M99;
The change of modal information by the interrupt program is invalidated and the original modal information is not restored. With interrupt type 1, however, if the interrupt program contains a move or miscellaneous function (MSTB) command, the original modal information is not restored.
Returning with M99P__;
The original modal information is updated by the change in the interrupt program even after returning to the main program. This is the same as in returning with M99P__; from a program called by M98.
Main program being executed
User macro interrupt signal (UIT)
Modal before interrupt is restored.
Modal modified by interrupt program remains effective.
Interrupt program
(Modal change)
M96Pp1 ; Op1 ;
M99(p2) ;
Np2 ;
(With Pp2 specified)
Modal information affected by user macro interrupt
13. Program Support Functions 13.12 Macro Interrupt ; M96, M97
387
Modal information variables (#4401 to #4520)
Modal information when control passes to the user macro interrupt program can be known by reading system variables #4401 to #4520. The unit specified with a command applies.
System variable Modal information #4401 to #4421 G code (group 01 to group 21) } Some groups are not used. #4507 D code #4509 F code #4511 H code #4513 M code #4514 Sequence number #4515 Program number (Note 1) #4519 S code #4520 T code
The above system variables are available only in the user macro interrupt program. If they are used in other programs, program error (P241) results. (Note 1) The programs are registered as files. When the program No. (file name) is read with
#4515, the character string will be converted to a value. (Example 1) The file name «123» is the character string 031, 032, 033, so the value
will be (031-030)*100 + (032-030)*10 + (033-030) = 123.0. Note that if the file name contains characters other than numbers, it will be
«blank». (Example 2) If the file name is «123ABC», characters other than numbers are included
in the file name; so, the result will be «blank».
M code for control of user macro interrupt
The user macro interrupt is controlled by M96 and M97. However, these commands may have been used for other operation. To be prepared for such case, these command functions can be assigned to other M codes. (This invalidates program compatibility.) User macro interrupt control with alternate M codes is possible by setting the alternate M code in parameters «#1110 M96_M» and «#1111 M97_M» and by validating the setting by selecting parameter «#1109 subs_M». (M codes 03 to 97 except 30 are available for this purpose.) If the parameter «#1109 subs_M» used to enable the alternate M codes is not selected, the M96 and M97 codes remain effective for user macro interrupt control. In either case, the M codes for user macro interrupt control are processed internally and not output to the outside.
13. Program Support Functions 13.12 Macro Interrupt ; M96, M97
388
Parameters
Refer to the Setup Manual for details on the setting methods. (1) Subprogram call validity «#1229 set 01/bit 0»
1 : Subprogram type user macro interrupt 0 : Macro type user macro interrupt
(2) Status trigger mode validity «#1112 S_TRG» 1 : Status trigger mode 0 : Edge trigger mode
(3) Interrupt type 2 validity «#1113 INT_2» 1 : The executable statements in the interrupt program are executed after completion of
execution of the current block. (Type 2) 0 : The executable statements in the interrupt program are executed before completion of
execution of the current block. (Type 1) (4) Validity of alternate M code for user macro interrupt control «#1109 subs_M»
1 : Valid 0 : Invalid
(5) Alternate M codes for user macro interrupt Interrupt enable M code (equivalent to M96) «#1110 M96_M» Interrupt disable M code (equivalent to M97) «#1111 M97_M» M codes 03 to 97 except 30 are available.
Restrictions
(1) If the user macro interrupt program uses system variables #5001 and after (position
information) to read coordinates, the coordinates pre-read in the buffer are used. (2) If an interrupt is caused during execution of the tool radius compensation, a sequence number
(M99P__;) must be specified with a command to return from the user macro interrupt program. If no sequence number is specified, control cannot return to the main program normally.
13. Program Support Functions 13.13 Tool Change Position Return ; G30.1 to G30.6
389
13.13 Tool Change Position Return; G30.1 to G30.6
Function and purpose
By specifying the tool changing position in a parameter «#8206 TOOL CHG. P» and also specifying a tool changing position return command in a machining program, the tool can be changed at the most appropriate position. The axes that are going to return to the tool changing position and the order in which the axes begin to return can be changed by commands.
Command format
(1) The format of tool changing position return commands is as follows.
G30. n; n = 1 to 6 : Specify the axes that return to the tool changing position and the order in
which they return.
For the commands and return order, see next table.
Command Return order G30.1 Z axis X axis Y axis ( added axis) G30.2 Z axis X axis Y axis ( added axis) G30.3 Z axis Y axis X axis ( added axis) G30.4 X axis Y axis Z axis ( added axis) G30.5 Y axis X axis Z axis ( added axis) G30.6 X axis Y axis Z axis ( added axis)
(Note 1) An arrow ( ) indicates the order of axes that begin to return. An period ( ) indicates that the axes begin to return simultaneously. (Example : «Z axis X axis, Y axis» indicate that the Z axis returns to the tool changing position, then the X and Y axes does.)
(2) The tool changing position return on/off for the added axis can be set with parameter «#1092
Tchg_A» for the added axis. Note, however, that the added axis always return to the tool changing position only after the
standard axes complete returning (see the above table). The added axis alone cannot return to the tool changing position.
(3) When the axis address is commanded in the same block as the tool change position return
command, the program error (P33) will occur.
13. Program Support Functions 13.13 Tool Change Position Return ; G30.1 to G30.6
390
Example of operates
(1) The figure below shows an example of how the tool operates during the tool change position
return command. (Only operations of X and Y axes in G30.1 to G30.3 are figured.)
G30.3
G30.2
G30.1
Tool changing position
Y
X
(a) G30.1 command: The Z axis returns to the tool changing position, then the X and Y axes
simultaneously do the same thing. (If tool changing position return is on for an added axis, the added axis also returns to the tool changing position after the X, Y and Z axes reach the tool changing position.)
(b) G30.2 command: The Z axis returns to the tool changing position, then the X axis does the
same thing. After that, the Y axis returns to the tool changing position. (If tool changing position return is on for an added axis, the added axis also returns to the tool changing position after the X, Y and Z axes reach the tool changing position.)
(c) G30.3 command: The Z axis returns to the tool changing position, then the X axis does the
same thing. After that, the X axis returns to the tool changing position. (If tool changing position return is on for an added axis, the added axis also returns to the tool changing position after the X and Z axes reach the tool changing position.)
(d) G30.4 command: The X axis returns to the tool changing position, then the Y axis and Z
axis simultaneously do the same thing. (If tool changing position return is on for an added axis, the added axis also return to the tool changing position after the X, Y and X axes reach the tool changing position.)
(e) G30.5 command: The Y axis returns to the tool changing position, then the X and Z axes
return to the tool changing position simultaneously. (If tool changing position return is on for an added axis, the added axis also returns to the tool changing position after the X, Y and Z axes reach the tool changing position.)
(f) G30.6 command: The X, Y and Z axes return to the tool changing position simultaneously.
(If tool changing position return is on for an added axis, the added axis also returns to the tool changing position after the X, Y and Z axes reach the tool changing position.)
13. Program Support Functions 13.13 Tool Change Position Return ; G30.1 to G30.6
391
(2) After all necessary tool changing position return is completed by a G30.n command, tool
changing position return complete signal TCP (XC93) is turned on. When an axis out of those having returned to the tool changing position by a G30.n command leaves the tool changing position, the TCP signal is turned off. With a G30.1 command, for example, the TCP signal is turned on when the Z axis has reached the tool changing position after the X and Y axes did (after the additional axis did if additional axis tool change position return is valid). The TCP signal is then turned off when the X or Y axis leaves the position. If tool changing position return for added axes is on with parameter «#1092 Tchg_A», the TCP signal is turned on when the added axis or axes have reached the tool changing position after the standard axes did. It is then turned off when one of the X, Y, Z, and added axes leaves the position.
Work program G30.3; G00X-100. T02; Arrival of Z axis to tool changing position Arrival of X, Y axes to tool changing position Arrival of added axis to tool changing position Tool changing position return complete signal (TCP)
[TCP signal output timing chart](G30.3 command with tool changing position return for added axes set on)
(3) When a tool changing position return command is issued, tool offset data such as for tool
length offset and tool radius compensation for the axis that moved is canceled. (4) This command is executed by dividing blocks for every axis. If this command is issued during
single-block operation, therefore, a block stop occurs each time one axis returns to the tool changing position. To make the next axis return to the tool changing position, therefore, a cycle start needs to be specified.
13. Program Support Functions 13.14 Normal Line Control ; G40.1/G41.1/G42.1
392
13.14 Normal Line Control ; G40.1/G41.1/G42.1
Function and purpose
If the C axis is set as the normal line control axis, the C axis (rotation axis) turning will be controlled so that the tool constantly faces the normal line direction control in respect to the XY axis movement command during program operation. At the block seams, the C axis turning is controlled so that the tool faces the normal line direction at the next block’s start point.
C axis turning
Tool end position
C axis center (rotation axis)
During arc interpolation, the rotation axis turning is controlled in synchronization with the operation of arc interpolation.
C axis center (rotation axis)
Tool end position
Tool
The normal line control I and II can be used according to the C axis turn direction during normal line control. This is set by the parameters.
Normal line control type Turning direction Turning speed Turning speed
in arc interpolation Type I
(#1524 C_type=0) Direction that is 180 or less (shortcut direction)
Parameter speed (#1523 C_feed)
Speed that the program path follows the F command
Type II (#1524 C_type=1)
As a principle, the commanded direction Feedrate Speed that the tool nose
follows the F command
13. Program Support Functions 13.14 Normal Line Control ; G40.1/G41.1/G42.1
393
Command format
G40.1 X__ Y__ F__ ; G41.1 X__ Y__ F__ ; G42.1 X__ Y__ F__ ; G40.1 : Normal line control cancel G41.1 : Normal line control left ON G42.1 : Normal line control right ON X : X axis end point coordinates Y : Y axis end point coordinates F : Feedrate
The axis No. for the normal line control axis is designated with the parameter (#1522 C_axis). Normal line control is carried out in respect to the axis movement direction of the selected plane. G17 plane X-Y axes G18 plane Z-X axes G19 plane Y-Z axes
Detailed description
(1) Definition of C axis turning direction
The C axis angle is 0 (degree) when the tool is facing the +X direction. The counterclockwise direction turning is + (plus), and the clockwise direction turning is (minus).
(2) C axis turning operation in respect to movement command (a) Start up
After the normal line control axis turns to a right angle of the advance direction at the start point of the normal line control command block, the axis of the selected plane is moved. Note that the normal line control axis at the start up turns in the direction that is 180 or less (shortcut direction) in both the normal line control type I and II.
(b) During normal line control mode
1. Block seam
No tool radius compensation
After the C axis is turned to be at a right angle of the movement of selected plane in the next block, that block is moved.
With tool radius compensation
If tool radius compensation is applied, normal line control is carried out along the path to which the tool radius compensation is applied.
2. During block movement
The C axis angle is kept constant during the linear command, and the C axis does not turn. During the arc command, the C axis turns in synchronization with the operation of the arc interpolation.
(c) Cancel
The C axis does not turn, and the axis movement of the selected plane by the program command is carried out.
13. Program Support Functions 13.14 Normal Line Control ; G40.1/G41.1/G42.1
394
(3) Normal line control temporally cancel
During normal line control, the turning operation for the normal line control axis is not carried out at the seam of the block that the movement amount is smaller than that set with the parameter (#1535 C_leng) and its previous block.
(Note) Since operation fractions are created by calculating the intersection point of two segments, the turning operation may be carried out or not when the parameter (#1535 C_leng) and the segment length are equal.
(4) Normal line control axis turning direction at block seam
The normal line control axis turning direction at block seam differs according to the normal line control type I or II. The turning angle is limited by the angle set with the parameter (#1521 C_min).
Item Type I Type II Normal line control axis turning direction at block seam
Direction that is 180 or less. (shortcut direction)
G41.1 : — direction (CW) G42.1 : + direction (CCW)
Normal line control axis turning angle at block seam
when | | < is applied, turning is not performed.
: Turning angle : Parameter (#1521 C_min)
When the turning angle is 180, the turning
direction is indefinite regardless of the command mode.
[G41.1/G42.1 When the normal line control axis is in 0]
No turning
—
0180
270
90 Normal line control axis turning (CCW)
Normal line control axis turning (CW)
when | | < is applied, turning is not performed.
: Turning angle : Parameter (#1521 C_min)
In the following cases, an operation error
(0118) will occur.
< 180 —
180 + < 360 — [G41.1 When the normal line control axis is in 0]
No turning
—
0180
270
90
Normal line control axis turning
Operation error (0118)
180-
[G42.1 When the normal line control axis is in 0]
No turning
—
0180
270
90
180 +
Normal line control axis turning
Operation error (0118)
13. Program Support Functions 13.14 Normal Line Control ; G40.1/G41.1/G42.1
395
(a) Normal line control type I Normal line control axis
turning angle at block seam: G41.1 G42.1
1. — < <
—
0 180
270 (-90)
90
No turning
No turning
2. < 180
0 180
270 (-90)
90
3. 180 360-
360 —
0 180
270 (-90)
90
Shortcut direction
Shortcut direction
13. Program Support Functions 13.14 Normal Line Control ; G40.1/G41.1/G42.1
396
(b) Normal line control type II Normal line control axis
turning angle at block seam: G41.1 G42.1
1. — < <
—
0 180
270 (-90)
90
No turning
No turning
2. < 180-
0 180
270 (-90)
90
180 —
Operation error (0118) (Note)
3. 180- 180+
180 —
0 180
270 (-90)
90
180 +
3. 180+ < 360-
360 —
0 180
270 (-90)
90
180 +
Operation error (0118) (Note)
(Note) Turning operation in the command direction is performed in the inside of the workpiece. Therefore, an operation error will occur.
13. Program Support Functions 13.14 Normal Line Control ; G40.1/G41.1/G42.1
397
(5) C axis turning speed
Turning speed at block seam (select from type 1 or type 2)
Item Type 1 Type 2 Normal line control axis turning speed at block seam
(a) Rapid traverse Dry run OFF
The rapid traverse rate (#2001 rapid) is applied. Normal line control axis turning speed f = Rapid traverse rate (Rapid traverse
override) (/min)
(a) Rapid traverse Dry run OFF
Normal line control axis turning speed f = F180/(R) (Rapid traverse override)
(/min) For R=0, the following expression is applied. Normal line control axis turning speed f = F (Rapid traverse override) (/min) F: Rapid traverse rate (#2001 rapid)
(mm/min) R: Parameter (#8041 C-rot.R) (mm)
(Length from normal line control axis center to tool nose)
(Note 1) If the normal line control axis
turning speed exceeds the rapid traverse rate (#2001 rapid), the speed is clamped to the rapid traverse rate.
Dry run ON The manual feedrate is applied. Normal line control axis turning speed f = Manual feedrate (Cutting feed
override) (/min) (Note 1) When the manual override valid is
ON, the cutting feed override is valid.
(Note 2) If the normal line control axis turning speed exceeds the cutting feed clamp speed (#2002 clamp), the speed is applied to the cutting feed clamp speed.
(Note 3) When the rapid traverse is ON, the dry run is invalid.
Dry run ON Normal line control axis turning speed f = F180/(R) (Cutting feed override)
(/min) For R=0, the following expression is applied. Normal line control axis turning speed f = F (Cutting feed override) (/min) F: Manual feedrate (mm/min) R: Parameter (#8041 C-rot.R) (mm)
(Length from normal line control axis center to tool nose)
(Note 1) When the manual override valid is ON, the cutting feed override is valid.
(Note 2) If the normal line control axis turning speed exceeds the rapid traverse rate (#2001 rapid), the speed is applied to the rapid traverse rate.
(Note 3) When the rapid traverse is ON, the dry run is invalid.
(Continued to the next page) (Continued to the next page)
13. Program Support Functions 13.14 Normal Line Control ; G40.1/G41.1/G42.1
398
Item Type 1 Type 2
Normal line control axis turning speed at block seam
(b) Cutting feed Dry run OFF
The normal line control axis turning speed set with the parameter (#1523 C_feed) is applied. Normal line control axis turning speed f = Parameter (#1523 C_feed) (Cutting
feed override) (/min) Dry run ON (Rapid traverse ON)
The cutting feed clamp speed (#2002 clamp) is applied. Normal line control axis turning speed f = Cutting feed clamp speed (/min)
Dry run ON (Rapid traverse OFF)
The manual feedrate is applied. Normal line control axis turning speed f = Manual feedrate (Cutting feed
override) (/min) (Note 1) When the manual override valid is
ON, the cutting feed override is valid.
(Note2) If the normal line control axis turning speed exceeds the cutting feed clamp speed (#2002 clamp), the speed is clamped to the cutting feed clamp speed.
F : Feed command speed
f : Normal line control axis turning speed = parameter (#1523 C_feed)
(Continued to the next page)
(b) Cutting feed The feedrate at the tool nose is the F command. The normal line control axis turning speed is the normal line control axis speed that follows this F command. Normal line control axis turning speed f = F180/(R) (Cutting feed override) (/min) For R=0, the following expression is applied. Normal line control axis turning speed f = F (/min) F: Feedrate command (mm/min) R: Parameter (#8041 C-rot.R) (mm)
(Length from normal line control axis center to tool nose)
(Note 1) If the normal line control axis
turning speed exceeds the cutting feed clamp speed (#2002 clamp), the speed is applied to the cutting feed clamp speed.
(Note2) When the dry run is ON, the normal line control axis turning speed is obtained with the same expression as the rapid traverse.
F: Feed command speed
Normal line control axis turning speed f =F*180/(*R)
R: Parameter (#8041 C-rot. R)
(Continued to the next page)
13. Program Support Functions 13.14 Normal Line Control ; G40.1/G41.1/G42.1
399
Item Type 1 Type 2
Normal line control axis turning speed during circular interpolation
The normal line control axis turning speed is the rotation speed obtained by feedrate F. Normal line control axis turning speed f = F180/(r) (degree/min)
F : Feed command speed (mm/min) r : Arc radius (mm)
(Note 1)
F: Feed command speed
r: Arc radius
Normal line control axis turning speed f =F*180/(*r)
The feedrate at the tool nose is the F command. The normal line control axis turning speed is the rotation speed that follows this F command.
Normal line control axis turning speed f = F180/((R+r)) (degree/min)
F : Feed command speed (mm/min) R : Parameter (#8041 C-rot. R) (mm)
Length from normal line control axis center to tool nose
r : Arc radius (mm)
F: Feed command speed
R: Parameter (#8041 C-rot. R) r: Arc radius
Normal line control axis turning speed f =F*180/(*(R+r))
(Note 1) If the normal line control axis turning speed exceeds the cutting feed clamp speed (#2002 clamp), the speed will be as follows; Normal line control axis turning speed = Cutting feed clamp speed. Moving speed during arc interpolation = The speed according to the normal line control axis turning speed
Automatic corner arc insertion function
During normal line control, an arc is automatically inserted into the corner in the axis movement of the plane selection. This function is for the normal line control type I. The radius of the arc to be inserted is set with the parameter (#8042 C-ins.R). This parameter can be read and write using the macro variable #1901. Normal line control is performed also during the interpolation for the arc to be inserted.
Parameter (#8042 C-ins.R)
13. Program Support Functions 13.14 Normal Line Control ; G40.1/G41.1/G42.1
400
The corner arc is not inserted into the straight line that is smaller than a linear-arc, arc-arc, linear-block with no movement, block with no movement-linear or radius of the arc to be inserted.
Corner R is not inserted.
During the radius compensation, the radius compensation is applied to the path that the corner arc is inserted into.
Parameter (#8042 C-ins.R) Radius compensation path
The stop point of the single block and block start interlock is as follows.
Stop point
The stop point of the cutting start interlock is as follows.
Stop point
Stop point
13. Program Support Functions 13.14 Normal Line Control ; G40.1/G41.1/G42.1
401
Precautions
(1) During normal line control, the program coordinates are updated following the normal line
control axis movement. Thus, program the normal line control with the program coordinate system.
(2) The normal line control axis will stop at the turning start position at the single block, cutting block start interlock and block start interlock.
(3) The C axis movement command is ignored during normal line control. (4) During C axis normal line control (during the G41.1 and G42.1 modal), the C axis workpiece
offset rewrite command (G92C_;) cannot be issued. The program error (P901) will occur if commanded.
(5) If mirror image is applied to either the 1-axis or 2-axis, the normal line control direction will be reversed.
(6) Designate the rotation axis for the normal line control axis (parameter (#1522 C_axis)). Designate so that the axis is not duplicated with the axis on the plane where normal line control is to be carried out. If an illegal axis is designated, the program error (P902) will occur when the program (G40.1, G41.1, G42.1) is commanded. The program error (P902) will also occur if the parameter (#1522 C_axis) is «0» when these codes are commanded.
(7) Depending on the model, this function cannot be used. (8) The movement of the normal line control axis is counted as one axis of number of
simultaneous contouring control axes. If the number of simultaneous contouring control axes exceeds the specification range by movement of the normal line control axis, the program error (P10) will occur.
Relation with other functions
Function name Notes
Uni-directional positioning
Normal line control is not applied.
Helical cutting Normal line control is applied normally. Spiral interpolation The start point and end point are not on the same arc, so normal line
control is not applied correctly. Exact stop check The operation will not decelerate and stop for the turning movement
of the normal line control axis. Error detect Error detect is not applied on the turning movement of the normal line
control axis. Override Override is applied on the turning movement by normal line control
axis. Coordinate rotation by program
Normal line control is applied to the shape after coordinate rotation.
Scaling Normal line control is applied to the shape after scaling. Mirror image Normal line control is applied to the shape after mirror image. Thread cutting Normal line control is not applied. Automatic reference position return
Normal line control is not applied.
Start position return Normal line control is not applied on the movement to the middle point position. If the base specification parameter «#1086 G0Intp» is 0, normal line control is applied to the movement from the middle point to a position designated in the program.
(Continued to the next page)
13. Program Support Functions 13.14 Normal Line Control ; G40.1/G41.1/G42.1
402
(Continued from the previous page)
Function name Notes High-accuracy control This cannot be commanded during normal line control. A program
error (P29) will occur. The normal line control command during high-accuracy control cannot also be issued. A program error (P29) will occur.
Spline This cannot be commanded during normal line control. A program error (P29) will occur. The normal line control command during spline cannot also be issued. A program error (P29) will occur.
High-speed High-accuracy control I/II
This cannot be commanded during normal line control. A program error (P29) will occur. The normal line control command during high-speed High-accuracy control I/II cannot also be issued. A program error (P29) will occur.
Cylindrical interpolation This cannot be commanded during normal line control. A program error (P486) will occur. The normal line control command during cylindrical interpolation cannot also be issued. A program error (P481) will occur.
Workpiece coordinate system offset
The workpiece coordinate system cannot be changed during normal line control. A program error (P29) will occur. The program parameter input (G10L2) cannot also be commanded. A program error (P29) will occur.
Local coordinate system offset
The local coordinate system cannot be changed during normal line control. A program error (P29) will occur.
Program restart The program including the normal line control command cannot be restarted. «E98 CAN’T RESEARCH» will occur.
Dry run The feedrate is changed by the dry run signal even in respect to the turning movement of the normal line control axis.
Chopping The axis cannot be used as the normal line control axis during the chopping command.
Graphic check The section turned by normal line control is not drawn. The path is drawn for the axes subjected to the graphic check.
G00 non-interpolation Normal line control is not applied. Pole coordinate interpolation
This cannot be commanded during normal line control. A program error (P486) will occur. The normal line control command during pole coordinate interpolation cannot also be issued. A program error (P481) will occur.
Exponential interpolation
If the normal line control axis is the same as the rotation axis of exponential interpolation, a program error (P612) will occur. If the normal line control axis is different from the rotation axis of exponential interpolation, an error will not occur, however normal line control is not applied.
Plane selection This cannot be commanded during normal line control. A program error (P903) will occur.
System variable The block end coordinate (#5001~) for the normal line control axis during normal line control cannot obtain a correct axis position.
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08
403
13.15 High-accuracy Control ; G61.1, G08
Function and purpose
This function aims to improve the error caused by the accuracy of the control system during machine machining. The parameter method and G code command method, which turn initial high-accuracy ON, are used to enter the high-accuracy control mode. Trouble such as the following occurred when using normal control: (1) Corner rounding occurred at linear and linear-connected corners because the following
command movement started before the previous command finished. (Refer to Fig. 1) (2) When cutting circle commands, an error occurred further inside the commanded path, and the
resulting cutting path was smaller than the commanded path. (Refer to Fig. 2)
Commanded path Commanded path
Actual path
Actual path
Fig. 1 Rounding at linear corners Fig. 2 Radius reduction error in circle commands
This function uses the following fix functions to minimize the increase in machining time while reducing the shape error. (1) Pre-interpolation acceleration/deceleration (linear acceleration/deceleration) (2) Optimum speed control (3) Vector accuracy interpolation (4) Feed forward (5) Arc entrance/exit speed control (6) S-pattern filter control
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08
404
Command format
G61.1 F__ ;
G61.1 F
: High-accuracy control mode ON : Feedrate command
The high-accuracy control mode is validated from the block containing the G61.1 command. The «G61.1» high-accuracy control mode is canceled with one of the G code group 13’s functions.
— G61 (Exact stop check mode) — G62 (Automatic corner override) — G63 (Tapping mode) — G64 (Cutting mode) — G08 P1 (High-accuracy control mode)
G08 P1(P0) ;
G08 P1 P0
: High-accuracy control mode : High-accuracy control mode start : High-accuracy control mode cancel
The «G08 P1» high-accuracy control mode is canceled with P0. Command G08P_ in an independent block. The decimal places below the decimal point are ignored for P address. (Note) G code group for in G08 is «0»; the priority is given to the function of the G code group 0 over
the function of the G code group 13. After «G08 P1» is commanded, G code group 13 is changed automatically to G64 (cutting) mode. Other command of «13» results in error. Even if high-accuracy control mode is canceled by «G08 P0» command, G64 (cutting) mode will not be changed. If you want to return to the function of G code group «13» when «G08 P1» has been commanded, command again after high-accuracy control mode is canceled.
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08
405
Detailed description
(1) Feedrate command F is clamped with #2110 Clamp(H-precision) (Cutting feedrate during
high-accuracy control mode for clamp function) set by the parameter. (2) Rapid traverse rate enables «#2109 Rapid(H-precision)» (Rapid traverse rate during
high-accuracy control mode) set by the parameter. (3) When the #2109 Rapid(H-precision) is set to 0, the movement follows 2001 rapid (rapid
traverse rate) set by the parameter. Also, when the setting value for #2110 Clamp(H-precision) is «0», the feedrate is clamped with #2002 clamp (cutting clamp speed) set by the parameter.
(4) The modal holding state of the high-accuracy control mode differs according to the combination of the base specification parameter «#1151 rstint» (reset initial) and «#1148 I_G611» (initial high-accuracy).
Parameter Default state Reset Emergency stop Emergency stop
cancel Block inter-
ruption
Block stop
NC alarm OT
R es
et in
iti al
(# 11
51 )
In iti
al h
ig h
ac cu
ra cy
(# 11
48 )
P ow
er O
N
R es
et 1
R es
et 2
R es
et &
re w
in d
E m
er ge
nc y
st op
s w
itc h
E xt
er na
l e m
er ge
nc y
st op
E m
er ge
nc y
st op
s w
itc h
E xt
er na
l e m
er ge
nc y
st op
M od
e ch
an ge
ov er
(a
ut om
at ic
/m an
ua lF
ee d
ho ld
S in
gl e
bl oc
k
S er
vo a
la rm
H /W
O T
OFF H H
ON OFF OFF
OFF OFF H
OFF
OFF H H ON
ON ON ON
ON H ON
H
H (hold): Modal hold ON: Switches to high-accuracy mode
As for G61.1, the mode is switched to the high-accuracy mode, even if the other modes (G61 to G64) are valid. OFF: The status of the high-accuracy mode is OFF.
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08
406
Pre-interpolation acceleration/deceleration
Acceleration/deceleration control is carried out for the movement commands to suppress the impact when the machine starts or stops moving. However, with conventional post-interpolation acceleration/deceleration, the corners at the block seams are rounded, and path errors occur regarding the command shape. In the high-accuracy control function mode, acceleration/deceleration is carried out before interpolation to solve the above problems. This pre-interpolation acceleration/deceleration enables machining on a machining path that more closely follows the command. The acceleration/deceleration time can be reduced because constant inclination acceleration/ deceleration is carried out. (1) Basic patterns of acceleration/deceleration control in linear interpolation commands
Acceleration/deceleration waveform pattern
Normal mode
Time
clamp
G1tL G1tL
S pe
ed o
f e ac
h ax
is
Time
clamp
G1t1 G1t1
S pe
ed o
f e ac
h ax
is
(a) Because of the constant time constant acceleration/deceleration, the rising edge/falling edge of the waveform becomes more gentle as the command speed becomes slower.
(b) The acceleration/deceleration time constant can be independently set for each axis. Linear type, exponential function type, or both can be selected. Note that if the time constant of each axis is not set to the same value, an error will occur in the path course.
#2002 clamp : G01 clamp speed #2007 G1tL : Linear type acceleration/ deceleration time constant #2008 G1t1 : Exponential type acceleration/ deceleration time constant
High-accuracy control mode
Time
clamp
G1btLG1btL
G1btL/2
G1bF
G1bF/2 C om
bi ne
d sp
ee d
G1btL/2
(a) Because of the constant inclination type linear acceleration/deceleration, the acceleration/deceleration time is reduced as the command speed becomes slower.
(b) The acceleration/deceleration time constant becomes one value (common for each axis) in the system.
#2002 clamp : G01 clamp speed #1206 G1bF : Target speed #1207 G1btL : Acceleration/deceleration time to target speed (Note) G1bF and G1btL are values for specifying
the inclination of the acceleration/ deceleration time; the actual cutting feed maximum speed is clamped by the «#2002 clamp» value.
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08
407
(2) Path control in circular interpolation commands
When commanding circular interpolation with the conventional post-interpolation acceleration/ deceleration control method, the path itself that is output from the CNC to the servo runs further inside the commanded path, and the circle radius becomes smaller than that of the commanded circle. This is due to the influence of the smoothing course droop amount for CNC internal acceleration/deceleration. With the pre-interpolation acceleration/deceleration control method, the path error is eliminated and a circular path faithful to the command results, because interpolation is carried out after the acceleration/deceleration control. Note that the tracking lag due to the position loop control in the servo system is not the target here. The following shows a comparison of the circle radius reduction error amounts for the conventional post-interpolation acceleration/deceleration control and pre-interpolation acceleration/deceleration control in the high-accuracy control mode.
R
R : Commanded radius (mm) R : Radius error (mm) F : Cutting feedrate (mm/min)
R
F
F
The compensation amount of the circle radius reduction error (R) is theoretically calculated as shown in the following table.
Post-interpolation acceleration/deceleration control
(normal mode)
Pre-interpolation acceleration/deceleration control
(high-accuracy control mode) Linear acceleration/deceleration
R = 1 2R
1 12
Ts2 + Tp2 F 60
2
Exponential function acceleration/deceleration
( ) R = 1 2R Ts2 + Tp2
F 60
2
Linear acceleration/deceleration
{ R = 1 2R Tp2 ( ) } 1 Kf 2 F
60
2
(a) Because the item Ts can be ignored by using the
pre-interpolation acceleration/deceleration control method, the radius reduction error amount can be reduced.
(b) Item Tp can be negated by making Kf = 1.
Ts : Acceleration/deceleration time constant in the CNC (s) Tp : Servo system position loop time constant (s) Kf : Feed forward coefficient
(Note) When a speed is set to #2110 Clamp (H-precision), which is the cutting clamp speed
parameter for the high-accuracy control mode, clamping will be carried out at that speed.
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08
408
Optimum speed control
(1) Optimum corner deceleration
By calculating the angle of the seam between blocks, and carrying out acceleration/ deceleration control in which the corner is passed at the optimum speed, highly accurate edge machining can be realized. When the corner is entered, that corners optimum speed (optimum corner speed) is calculated from the angle with the next block. The machine decelerates to that speed in advance, and then accelerates back to the command speed after the corner is passed. Corner deceleration is not carried out when blocks are smoothly connected. In this case, the criteria for whether the connection is smooth or not can be designated by the machining parameter «#8020 DCC ANGLE». When the corner angle is larger than the parameter «DCC ANGLE» for a linearlinear connection, or for a circle, etc., the acceleration V occurs due to the change in the direction of progress after the corner is passed at a speed V.
V
V Speed before entering the corner V Speed change at the corner
Speed after the corner is passed The corner angle V is controlled so that this V value becomes less than the pre-interpolation acceleration/ deceleration tolerable value set in the parameters («#1206 G1bF», «#1207 G1btL»). In this case the speed pattern is as follows.
Y axis
X axis
N01 G01X100.Y1.F500 ; N02 G01X100.Y-1.F500 ;
Y axis speed pattern
X axis speed pattern
Combined speed pattern Speed
Time V0
V0x
V0y
The optimum corner speed is represented by V0. V0 is obtained from the pre-interpolation acceleration/deceleration tolerable value (V’) and the corner angle (outside angle) .
To further reduce the corner speed V0 (to further improve the edge accuracy), the V0 value can be reduced in the machining parameter «#8019 R COMPEN».
V’ = G1bF G1btL
V0′ = V0 (100 — Ks)
100
V0 = V0x2 + V0y2
(Note 1) In this case, the cycle time may increase due to the increase in the time required for acceleration/ deceleration.
(Note 2) V0 can be increased by setting a negative value for the accuracy coefficient.
Ks: R COMPEN Speed
Time
Speed
Time
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08
409
The accuracy coefficient differs according to parameter «#8201 COMP CHANGE».
#8201 COMP CHANGE Accuracy coefficient used 0 #8019 R COMPEN 1 #8022 CORNER COMP
The corner speed V0 can be maintained at a set speed or more so that the corner speed does not drop too far. Set «#2096 crncsp (corner deceleration minimum speed)» for each axis, and make a composite speed so that the moving axis does not exceed this setting.
X axis setting value
Y axis setting value
Clamp value according to X axis
Corner deceleration speed
Speed is clamped
V
Corner deceleration speed
Speed is not clamped
Note that the speed is controlled with the optimum corner deceleration speed in the following cases. When the composite corner deceleration speed is less than the optimum corner deceleration
speed. When the corner deceleration minimum speed parameter setting for the moving axes is set
to «0» for even one axis.
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08
410
(2) Arc speed clamp
During circular interpolation, even when moving at a constant speed, acceleration is generated as the advance direction constantly changes. When the arc radius is large compared to the commanded speed, control is carried out at the commanded speed. However, when the arc radius is relatively small, the speed is clamped so that the generated acceleration does not exceed the tolerable acceleration/deceleration speed before interpolation, calculated with the parameters. This allows arc cutting to be carried out at an optimum speed for the arc radius.
F : Commanded speed (mm/min) R : Commanded arc radius (mm) : Angle change per interpolation unit V : Speed change per interpolation unit The tool is fed with the arc clamp speed F so that V does not exceed the tolerable acceleration/deceleration speed before interpolation V.
F
F
F
F
V
F R V 60 1000 (mm/min)
V = G1btL (ms)
G1bF (mm/min)
When the above F’ expression is substituted in the expression expressing the maximum logical arc radius reduction error amount R explained in the section «a) Pre-interpolation acceleration/deceleration», the commanded radius R is eliminated, and R does not rely on R.
R 1
2R {Tp2 (1 Kf2) } ( )2 F
60
1
2 {Tp2 (1 Kf2) } ( )
V’ 1000
60
R : Arc radius reduction error amount
Tp : Position loop gain time constant of
servo system
Kf : Feed forward coefficient
F : Cutting feedrate
In other words, with the arc command in the high-accuracy control mode, in logical terms regardless of the commanded speed F or commanded radius R, machining can be carried out with a radius reduction error amount within a constant value. To further lower the arc clamp speed (to further improve the roundness), the arc clamp speed can be lowered with the machining parameter «#8019 R COMPEN». In this case, speed control is carried out to improve the maximum arc radius reduction error amount R by the set percentage.
R’
R (100 — Ks)
100 (mm)
R’ : Maximum arc radius reduction error amount Ks : R COMPEN (%)
After setting the «R COMPEN», the above R’ will appear on the parameter screen.
Accuracy coefficient setting value
#8019 R COMPEN (0.078) 50
R’ (Note 1) The maximum arc radius reduction error amount R can be increased by setting a
negative value for the «accuracy coefficient». (Note 2) When the «R COMPEN» is set with positive value, the arc clamp speed will drop, so in a
machining program with many arc commands, the machining time will take longer.
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08
411
(Note 3) The «R COMPEN» is valid only when the arc speed clamp is applied. To reduce the radius
reduction error when not using the arc speed clamp, the commanded speed F must be lowered.
(Note 4) If the «accuracy coefficient» is not set (0), arc speed clamping will not be applied. (Note 5) The «accuracy coefficient» differs according to parameter «#8021 COMP CHANGE».
#8201 COMP CHANGE Accuracy coefficient used
0 #8019 R COMPEN 1 #8023 CURVE COMP
Vector accuracy interpolation
When a fine segment is commanded and the angle between the blocks is extremely small (when not using optimum corner deceleration), interpolation can be carried out more smoothly using the vector accuracy interpolation.
Commanded path
Vector accuracy interpolation
Feed forward control
With this function, the constant speed error caused by the position loop control of the servo system can be greatly reduced. However, as machine vibration is induced by the feed forward control, there are cases when the coefficient cannot be increased. In this case, use this function together with the smooth high gain (SHG) control function and stably compensate the delay by the servo system’s position loop to realize a high accuracy. As the response is smoother during acceleration/deceleration, the position loop gain can be increased.
(1) Feed forward control
Command during acceleration/ deceleration before interpolation
Command during acceleration/ deceleration after interpolation
Machine error compensation amount
Kp : Position loop gain Kv : Speed loop gain M : Motor S : Segment
Feed forward control
Detector
Kp
S
Kv M
+ ++
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08
412
(2) Reduction of arc radius reduction error amount using feed forward control
With the high-accuracy control, the arc radius reduction error amount can be greatly reduced by combining the pre-interpolation acceleration/deceleration control method above-mentioned and the feed forward control/SHG control. The logical radius reduction error amount R in the high-accuracy control mode is obtained with the following expression.
Feed forward control SHG control + Feed forward control R
1
2 R {T p 2 (1 K f2 ) } ( ) 2F
6 0
By setting Kf to the following value, the delay elements caused by the position loop in the servo system can be eliminated, and the logical R can be set to 0. Kf = 1 (Feed forward gain 100%) The equivalent feed forward gain to set Kf to 1 can
be obtained with the following expression.
100 1 1 50
2 2
fwd g_ PGN1 for conventional control 2 PGN1 for SHG control
The feed forward gain can be set independently for G00 and G01.
Path for post-interpolation acceleration/deceleration control method
Path for pre-interpolation acceleration/deceleration control method (Kf = 0)
Path for pre-interpolation acceleration/deceleration control method (Kf = 1)
R
R
F
(Note) If the machine vibrates when Kf is set to 1, Kf must be lowered or the servo system must
be adjusted.
R : Arc radius (mm) F : Cutting feedrate (mm/min) Tp : Position loop time constant (s) Kf : Feed forward coefficient (fwd_g/100)
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08
413
Arc entrance/exit speed control
There are cases when the speed fluctuates and the machine vibrates at the joint from the straight line to arc or from the arc to straight line. This function decelerates to the deceleration speed before entering the arc and after exiting the arc to reduce the machine vibration. If this is overlapped with corner deceleration, the function with the slower deceleration speed is valid. The validity of this control can be changed with the base specification parameter «#1149 cireft». The deceleration speed is designated with the base specification parameter «#1209 cirdcc».
(Example 1) When not using corner deceleration
G61.1 ;
N1 G01 X-10. F3000 ; N2 G02 X-5. Y-5. J-2.5 ; N3 G01 Y-10. ;
N1
N2
N3
N1 N2 N3 Commanded speed
Arc clamp speed
Arc deceleration speed
Speed
Time
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08
414
(Example 2) When using corner deceleration
G61.1 ;
N1 G01 X-10. F3000 ; N2 G02 X5. Y-5. I2.5 ; N3 G01 X10. ;
N1
N2 N3
N1 N2 N3
Corner deceleration speed
Commanded speed
Arc clamp speed
Arc deceleration speed
Speed
Time
S-pattern filter control
This control interpolates while smoothing the changes in the segments distributed to each axis element with vector accuracy interpolation. With this, the fluctuation amplified by feed forward control is reduced and the effect onto the machine is reduced. This can be set in the range of 0 to 200(ms) with the basic specification parameter #1568 SfiltG1 and #1569 SfiltG0. With #1570 Sfilt2, this also enables the acceleration/deceleration fluctuation to further smoothen.
F
T
Command to drive unit
Parameter setting value
F
T
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08
415
Circular error radius compensation control for each axis
When the roundness at the machine end is, compared to the reference circle, expanded at an axis creating an ellipsis state, compensation is carried out for each axis to make a perfect circle. The validity of this control can be changed with control parameter «#8108 R COMP Select». Note that «#8108 R COMP Select» is valid only when «#8107 R COMPENSATION» is set to «1». The compensation coefficient for each axis is designated with the axis specification parameter «#2069 Rcoeff».
(1) Compensation in each axis direction of arc
Machine end path
Commanded path
Machine end path
Commanded path
(2) Smooth compensation at entrance and exit
The compensation amount is gradually increased from the arc start point to the 90 position, and 100% compensation is reached at the 90 position. The compensation is gradually decreased from 90 before the end point, and 0% compensation is reached at the end point.
Machine end path
Commanded path
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08
416
Relation with other functions
(1) The modals must be set as shown below when commanding G08P1. Function G code
High-speed high-accuracy control II, High-speed machining cancel
G05 P0
Cylindrical interpolation cancel G07.1 High-accuracy control cancel G08 P0 Polar coordinate interpolation cancel G15 Tool radius compensation mode cancel G40 Normal line control cancel G40.1 Tool length compensation cancel G49 Programmable mirror image OFF G50.1 Mirror image with settings Cancel Mirror image with signals Cancel No macro modal call G67 Feed per revolution cancel G94 Constant surface speed control mode cancel G97 Interruption type macro mode M97
(2) An alarm will occur if high-accuracy control is commanded in the following modes.
During milling Program error (P481) During cylindrical interpolation Program error (P481) During polar coordinate interpolation Program error (P481) During normal line control Program error (P29)
(3) A program error (P29) will occur if the following commands are issued during the high-accuracy control mode. Milling Cylindrical interpolation Polar coordinate interpolation Normal line control
Precautions
(1) The «high-accuracy control» specifications are required to use this function.
If G61.1 is commanded when there are no specifications, a program error (P123) will occur. (2) Command G61.1 in an independent block. (3) The G61.1 command can be used when the basic parameter «#1267 ext03/bit0» is set to «0». If
G61.1 is commanded when the parameter is set to «1», a program error (P34) will occur. (4) This function may not be usable depending on the model. (5) The #1205 G0bdcc (G0 pre-interpolation) can be used with only one part system.
If the 2nd or later part system is set to the G0 acceleration/deceleration before interpolation, an error will occur.
(6) «#1568 SfiltG1», «#1569 SfiltG0» and «#1570 Sfilt2» cannot be changed from the screen during program operation. If these parameters is changed by «parameter input by program», these parameters are valid after the axes stop.
13. Program Support Functions 13.16 High-speed Machining Mode ; G05, G05.1
417
13.16 High-speed Machining Mode ; G05, G05.1 13.16.1 High-speed Machining Mode I,II ; G05 P1, G05 P2
Function and purpose
This function runs a machining program for which a freely curved surface has been approximated by fine segments at high speed. This is effective in increasing the speed of machining dies of a freely curved surface. G1 block fine segment capacity for 1mm segment
Mode Command Maximum feedrate when 1mm segment G1 block is executed
Standard mode G05 P0 16.8 m/min High-speed
machining mode I G05 P1 16.8 m/min
High-speed machining mode II
G05 P2 135.0 m/min
The above performance applies under the following conditions. 6-axis system (including spindle) or less 1-part system 3 axes or less commanded simultaneously in G01 Block containing only axis name and movement amount (Macro and variable command are
not included.) During G61.1 high-accuracy control mode, or during cutting mode (G64) During tool radius compensation cancel (G40) (Only in the high-speed machining mode II)
When the above conditions are not satisfied, the given feedrate may not be secured.
Command format
G05 P1 ; …….. High-speed machining mode I ON
G05 P0 ; …….. High-speed machining mode I OFF
G05 P2 ; …….. High-speed machining mode II ON
G05 P0 ; …….. High-speed machining mode II OFF
In addition to the G05 P0 command, the high-speed machining mode I is canceled with the command of High-speed machining mode II(G05 P2). Also, High-speed machining mode II can be canceled with the command of High-speed machining mode I.
13. Program Support Functions 13.16 High-speed Machining Mode ; G05, G05.1
418
Detailed description
(1) The override, maximum cutting speed clamp, single block operation, dry run, manual
interruption and graphic trace and high-accuracy control mode are valid even during the high-speed machining mode I/II.
(2) When using the high-speed machining mode II mode, set «BIT1» of the parameter «#1572 Cirorp» to «1» to eliminate the speed fluctuation at the seams of the arc and straight line or arc and arc.
Example of program (High-speed machining mode I)
G28 X0. Y0. Z0. ; G91 G00 X-100. Y-100. ; G01 F10000 ; G05 P1 ; —— High-speed machining mode I ON : X0.1 Y0.01 ; X0.1 Y0.02 ; X0.1 Y0.03 ; : G05 P0 ; —— High-speed machining mode I OFF M30 ;
13. Program Support Functions 13.16 High-speed Machining Mode ; G05, G05.1
419
Restrictions
(1) If G05 P1(P2) is commanded when the option for high-speed machining mode I/(II) is not
provided, a program error (P39) will occur. (2) The automatic operation process has the priority in the high-speed machining mode I/II , so the
screen display, etc., may be slowed down. (3) The speed will decelerate once at the G05 command block, so turn ON and OFF when the tool
separates from the workpiece. (4) When carrying out operation in the high-speed machining mode I/II by communication or tape
operation, the machining speed may be suppressed depending on the program transmission speed limit.
(5) Command the G05 command in an independent block. (6) A decimal point cannot be used for the P address in the G05 command block. (7) Only P0, P1, and P2 are valid as P address in the G05 command block.
If an address other than P is commanded in the G05 block, a program error (P35) will occur. If there is no P command, a program error (P33) will occur.
(8) The machining speed may be suppressed depending on the number of characters in a designated block.
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1
420
13.17 High-speed High-accuracy Control ; G05, G05.1 13.17.1 High-speed High-accuracy Control I, II
Function and purpose
This function runs a machining program that approximates a freely curved surface with fine segments at high speed and high accuracy. This is effective in increasing the speed of machining dies of a freely curved surface. Simultaneous 3-axis fine segment capacity for 1mm segment
Performance of the fine segment execution High-speed high-accuracy control I
mode Without radius compensation
With radius compensation
Restriction in the program
Invalid 16.8m/min 16.8m/min No Valid 33.6m/min 33.6m/min Yes
Command format
G05.1 Q1 ; …….. High-speed high-accuracy control I ON G05.1 Q0 ; …….. High-speed high-accuracy control I OFF
G05 P10000 ; … High-speed high-accuracy control II ON G05 P0 ; ……….. High-speed high-accuracy control II OFF
(Note 1) The high-speed high-accuracy mode l and II can not be used at the same time. (Note 2) G05.1 Q1 (high-speed high-accuracy mode I) and G05 P10000 (high-speed
high-accuracy mode II) are valid when the parameter «#1267 ext03/bit0» is ON.
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1
421
Detailed description
(1) The high-speed high-accuracy control I / II can be used during computer link, tape, MDI, IC
card or memory operation. (2) The override, maximum cutting speed clamp, single block operation, dry run, handle interrupt
and graphic trace are valid even during the high-speed high-accuracy control I / II modal. (3) The machining speed may drop depending on the number of characters in one block. (4) The high-speed high-accuracy control I / II function automatically turns the high-accuracy
control mode ON. For high-accuracy control function, refer to 13.14 High-accuracy control (5) Turn the tool radius compensation command ON and OFF during the high-speed
high-accuracy control I / II mode. If the high-speed high-accuracy control I / II mode is turned OFF without turning the tool radius compensation OFF, program error (P34) will occur.
(6) Turn the high-speed high-accuracy control I / II mode OFF before commanding data other than the data listed above.
(7) When using the high-speed high-accuracy control II mode, set parameter «#1572 Cirorp» to «1» to eliminate the speed fluctuation at the seams of the arc and straight line or arc and arc.
(8) Feedrate command (F) is clamped with the «#2110 Clamp (H-precision)» (Cutting feed clamp speed for high-accuracy control mode) set with parameter.
(9) «#2109 Rapid (H-precision)» (Rapid traverse speed for high-accuracy control mode) set with parameter will be valid for the rapid traverse speed.
(10) When «#2109 Rapid (H-precision)» is set to «0», movement is performed with «#2001 rapid» (Rapid traverse rate) set with parameter. Also, when «#2110 Clamp (H-precision)» is set to «0», clamp will be made with «#2002 clamp» (Cutting clamp speed) set with parameter.
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1
422
Additional functions when high-speed high-accuracy control 2 mode is ON
(1) Fairing If there is a protruding path (zigzagging path) shorter than the parameter setting values in the machining program generated with a CAM, etc., this function can be used to eliminate the protruding path smaller than the setting value so that the front and back paths are smoothly connected. This function is valid only for continuous linear commands (G1).
Related parameter Details #8033 Fairing ON 0: Fairing invalid
1: Execute fairing for the protruding block #8029 Fairing L Execute fairing for the shorter block than this setting value
Path before/after fairing execution
After fairing Before fairing
If there is any protruding path after fairing, fairing is repeated.
Path in repetitive fairing executions
Before fairing After first fairing After final fairing
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1
423
(2) Acceleration clamp speed
With the cutting feed clamp speed during the high-speed high-accuracy control 2 mode, when the following parameter is set to «1», the speed is clamped so that the acceleration generated by each block movement does not exceed the tolerable value. This function clamps the speed optimally even at a section where «angle change at each block is small but entire curvature is large» such as shown below. The tolerable acceleration value is calculated from the parameter «#1206 G1bF» and «#1207 G1btL» setting values. (Tolerable acceleration = #1206/#1207)
Related parameter Details
#8034 AccClampt ON 0: Clamp the cutting speed with parameter «#2002 clamp» or the corner deceleration function.
1: Clamp the cutting speed with acceleration judgment.
Speed control by curvature
If the tool moves along the large curvature section without deceleration, a large acceleration is generated resulting in a path error by curving inward.
R
(Note) When a speed is set in «#2109 Clamp(H-precision)», clamp is executed at that speed. When the setting value is 0,clamp is executed with «#2002 clamp».
(3) Corner deceleration in high-speed mode
During high-accuracy control, if the angle is large between the adjacent blocks in the machining program, this function, conventionally, automatically decelerates so that the acceleration generated when passing through the corner is within the tolerable value. If a small block is inserted at the corner section in the machining program generated with the CAM, etc., the corner passing speed will not match the periphery. This can affect the machining surface. If this type of small block is inserted when performing corner deceleration in the high-speed mode, the corner will be largely judged by the parameter settings. The small block is excluded when the angle is judged, but is not excluded from the actual movement command.
Related parameter Details
#8036 CordecJudge 0: Judge the corner from the angle of the neighboring block. 1: Judge the corner from the angle of the neighboring block,
excluding the minute blocks. #8037 CorJudgeL Exclude shorter block than this setting value.
When «#8036 CordecJudge» is set to «1», corner deceleration is realized without an influence of fine blocks.
High-speed mode corner deceleration
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1
424
Precautions
(1) High-speed high-accuracy control I and II are the optional functions. If «G05.1 Q1» or «G05
P10000″ is commanded when the option is not provided, a program error (P39) will occur. (2) The automatic operation process has the priority in the high-speed high-accuracy control I/II
modal, so the screen display, etc., may be delayed. (3) The speed will decelerate once at the «G05.1 Q1″/»G05.1 Q0» and the «G05 P10000″/»P05 P0»
command block, so turn ON and OFF when the tool separates from the workpiece. (4) If an address other than G/Q or P/N is commanded in the «G05.1 Q1″/»G05.1 Q0» and «G05
P10000″/»G05 P0″ command block, a program error (P33) will occur. (5) Command the «G05.1 Q1″/»G05.1 Q0» and the «G05 P10000″/»G05 P0» command in an
independent block. (6) When carrying out high-speed high-accuracy control I/II operation during tape operation, the
machining speed may be suppressed depending on the program transmission speed and the number of characters in one block.
(7) If there is no Q or P command in the G05.1 or G05 command block, a program error (P33) will occur.
(8) A decimal point cannot be used in the Q or P command. (9) If the high-speed high-accuracy control I command is issued in the high-speed high-accuracy
control II modal, a program error (P34) will occur. (10) If the high-speed high-accuracy control II command is issued in the high-speed high-accuracy
control I modal, a program error (P34) will occur. (11) Variable commands and user macros cannot be used in the high-speed high-accuracy control
II modal. (12) Fairing function is valid for the continuous linear command (G1). Fairing is not possible in the
case below. G02
G01G02
(13) The G codes for this function are valid when the parameter «#1267 ext03/bit0» setting value is
«0». If G05.1 Q1 is commanded when this setting value is «0», a program error (P34) will occur.
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1
425
Relation with other functions
(1) The modal state must be as shown below when commanding G05.1 Q1 and G05 P10000. Program error (P34) will occur if the conditions are not satisfied. When commanding a SSS control, refer to 3.16.2 SSS control for details.
Function G code Tool radius compensation cancel G40 Tool length compensation cancel G49 For only mode I G command mirror image cancel G50.1 Mirror image cancel with parameter settings Cancel
Mirror image cancel with signals Cancel Cutting mode G64 User macro modal call cancel G67 Programmable coordinate rotation mode OFF G69
Fixed cycle cancel G80 Feed per minute G94 Constant surface speed control OFF G97 User macro interrupt cancel M97
Although G05.1 Q can be commanded in the modals listed below, correct movement may not be guaranteed.
Function G code Exact stop check mode G61 Automatic corner override G62 Tapping mode G63 Feed per revolution G95 Constant surface speed G96
(2) The following data can be commanded while the high-speed high-accuracy control I/II mode is
ON. Program error will occur if other data is commanded. High-speed
high-accuracy mode Function
I II
G code
Positioning G00 Cutting feed G01 G02 G03 Helical interpolation G02 G03 Plane selection G17 G18 G19 Tool radius compensation G40 G41 G42 Tool length compensation — G43 G44 G49 Programmable mirror image G50.1 G51.1 Mirror image with parameter settings — — — Mirror image with signals — — — Absolute command G90 Incremental command G91 Workpiece coordinate system setting — G92 Workpiece coordinate system selection — G54~G59 Machine coordinate system command — G53
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1
426
(Note 1) M96 and M97 cannot be used. (High-speed high-accuracy control II only)
High-speed high-accuracy
mode Function
I II
G code
Subprogram call M98
External subprogram call M198 Programmable parameter input — G10 L50 Programmable compensation amount input
— G10 L10
High-speed high-accuracy control I cancel
— G05.1 Q0
High-speed high-accuracy control II cancel
— G05 P0
Spline control — G05.1 Q2 G05.1 Q0 F code command Fxxx Sequence No. command Nxxx Comment command ( ) Optional block skip / Miscellaneous function (Note 1) Mxxx Sxxx Txxx Bxxx I/J/K/R command for circular interpolation
I J K R
Axis movement command X Y Z etc.
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1
427
13.17.2 SSS Control
Function and purpose
With conventional high-accuracy control, the angle between two blocks is compared with the corner deceleration angle to determine whether to execute corner deceleration between the blocks. This can cause the speed to suddenly change between the blocks with an angle close to the corner deceleration angle, resulting in scratches or streaks. With SSS (Super Smooth Surface) control, the user can predict the optimum machining speed, using the large area of path information. Comparing to the conventional high-accuracy control function, SSS control has more advanced features so that smoother workpiece cutting surface is realized. The followings are some of the features available in SSS control.
(1) Speed fluctuation caused by the effect of the machining-disturbing blocks (minute stepping or waviness) is suppressed. Thus, scratches caused by these blocks are reduced.
(2) Even if corner deceleration is not required, the speed is clamped if the predicted acceleration is high.
Furthermore, the machining time can be reduced in machining applications having many corners.
Conventional optimum corner deceleration
Feedrate
Time
Do not decelerate
Feedrate
Time
SSS control
Decelerate according to angle
When corner deceleration angle is or less
Feedrate
Time
When corner deceleration angle is or more
Feedrate
Time
=
The length of the path direction recognized with SSS control can be adjusted with the machining parameter «#8091 StdLength». The range is increased as the setting value increases, and the effect of the error is reduced. (Note) This function is an option. The high-speed high-accuracy control II option is required to
use this function.
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1
428
Detailed description
(1) The following procedures are followed to use SSS control. (a) Turn the following parameters ON beforehand. Basic specification parameter «#1267 ext03/bit0» Machining parameter «#8090 SSS ON» (b) Command «G05 P10000 ;» (high-speed high-accuracy control II ON).
SSS control is valid until «G05 P0 ;» (high-speed high-accuracy control II OFF) is commanded.
(2) The SSS control can be used during computer link, tape, MDI, IC card or memory operation. (3) The machining speed may drop depending on the number of characters in one block. (4) To command data other than the valid command data, turn the SSS control mode OFF first.
Relation with other functions
(1) The modals must be set as shown below when SSS control starts. A program error (P34) will occur if these conditions are not satisfied.
Modal state
Function Mode Tool radius compensation mode G40 Programmable mirror image G50.1 Cutting mode G64 Macro modal call mode G67 Programmable coordinate rotation mode G69 Canned cycle mode G80 Per-rotation feed G94 Constant surface speed control mode G97 Interrupt type macro mode M97
Status other than modals Function Status
Parameter mirror image OFF External mirror image OFF
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1
429
(2) The following functions can be commanded during the SSS control mode.
A program error will occur if any other function is commanded. During G code command: Program error (P34) Other cases: Program error (P33)
Function Command
Positioning G00 Cutting feed G01 G02 G03 Helical interpolation G02 G03 Spiral interpolation G02.1 G03.1 Plane selection G17 G18 G19 Tool radius compensation G40 G41 G42 Programmable mirror image G50.1 G51.1 Absolute command G90 Incremental command G91 Subprogram call M98 External subprogram call M198 High-speed high-accuracy control II cancel
G05 P0
Spline control G05.1 Q2 G05.1 Q0 F code command Fxxx Sequence No. command Nxxx Comment command ( ) Optional block skip / Auxiliary function (Note 1) Mxxx Sxxx Txxx Bxxx I, J, K, R command for circular interpolation
I J K R
Axis movement data X Y Z etc. (3) The F1-digit command function cannot be used. (4) M96 and M97 cannot be used. (5) The override, maximum cutting speed clamp, signal block operation and graphic trace are valid
even during the SS control mode. (6) The tool radius compensation command should not be used during the SSS control mode. (7) Turn the tool radius compensation command ON and OFF during the SSS control mode.
If the SSS control mode is turned OFF before the tool radius compensation is turned OFF, a program error (P34) will occur.
(8) The geometric IB command is invalid during SSS control, and will be handled as a normal arc command.
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1
430
Parameter standard values
The standard values of the parameters related to SSS control are shown below.
(1) Machining parameters
# Item Standard value 8019 R COMP 0 8020 DCC ANGLE 10 8021 COMP CHANGE 1 8022 CORNER COMP 0 8023 CURVE COMP -20 8029 Fairing L 0 8033 Fairing ON 0 8034 AccClamp ON 0 8036 CordecJudge 0 8037 CorJudgeL 0
(Note) Reference items for adjusting the parameter
The relation of each parameter, the accuracy and the speed is shown below. The accuracy and speed required for machining can be adjusted with these settings. When adjusting the parameters, adjust the values within the range in which the machine does not vibrate.
Parameter Adjustment target Effect
#8022 CORNER COMP Accuracy at corner section
Large setting = Accuracy improves, speed drops
#8023 CURVE COMP Accuracy at curve section
Large setting = Accuracy increases, speed drops
#8092 ClampCoeff Accuracy at curve section
Large setting = Accuracy drops, speed increases (Note) Usually use the standard value and adjust with «#8023».
(2) Basic specification parameters
# Item Standard value 1148 I_G611 Initial high accuracy 0 1205 G0bdcc G0 before interpolation 0 1206 G1bf Acceleration/deceleration before
interpolation Maximum speed —
1207 G1btL Acceleration/deceleration before interpolation Time constant
—
1209 Cirdcc Arc deceleration speed — 1267 ext03/bit0 G code type 1 1572 Cirorp Arc command overlap 0 1568 SfiltG1 G1 soft acceleration/deceleration filter 0 1569 SfiltG0 G0 soft acceleration/deceleration filter 0 1570 Sfilt2 Soft acceleration/deceleration filter 2 0
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1
431
(3) Axis specification parameters
# Item Standard value 2010 fwd_g Feed forward gain 70 2068 G0fwdg G00 feed forward gain 70 2096 crncsp Minimum corner deceleration speed 0
Restrictions
(1) Pre-reading is executed during SSS control, so a program error could occur before the block
containing the error is executed. (2) Do not correct the buffer during SSS control. The operation will not be guaranteed if the buffer
is corrected. (3) If automatic/manual simultaneous or automatic handle interrupt are used during SSS control,
the machining accuracy will not be guaranteed. (4) During SSS control, if override is set to «0» in the single block stop state, the «M01 operation
error 0102 override zero» will occur. (5) If a fine arc command is issued during SSS control, it may take longer to machine. (6) A program error (P33) will occur if external input mirror image is applied during SSS control. (7) The same path as single block operation will be used during graphic check. (8) The line under the cutting feedrate and arc command block are subjected to the speed control
in the SSS control. However, rotary axis command block is not subjected to SSS control. In the command blocks that are not subjected to speed control, decelerates first and automatically switches the SSS control ON and OFF
13. Program Support Functions 13.18 Spline; G05.1
432
13.18 Spline; G05.1 Function and purpose
This function automatically generates a spline curve that passes through a sequence of points commanded by the fine segment machining program, and interpolates the path along this curve. This allows highly accurate machining at a high speed. The spline function can be commanded when the machining parameter «#8025 SPLINE ON» is set to 1 in the high-speed high-accuracy control function II mode (between G05P10000 and G05P0). The following explanation is limited to the spline function in the high-speed high-accuracy control function II mode.
Command format
G05.1Q2X0Y0Z0 ; Spline mode ON G05.1Q0 ; Spline mode OFF
Example of program
: G91 ; G05 P10000 ; …………………….. High-speed high-accuracy control function II mode ON : G05.1 Q2 X0 Y0 Z0 ; …………… Spline mode ON G01 X1000 Z-300 F1000 ; X1000 Z-200 ; Y1000 ; X-1000 Z-50 ; X-1000 Z-300 ; G05.1 Q0 ; …………………………. Spline mode OFF : G05 P0 ;…………………………….. High-speed high-accuracy control function II mode OFF :
(1) The spline function carries out spline interpolation when the following conditions are all
satisfied. If the following conditions are not satisfied, the spline function is canceled once, and it is judged whether to carry out new spline from the next block. When the block length is shorter than the machining parameter «#8030 MINUTE LENGTH». When the movement amount is not 0. When one of the following modes is entered.
G01: Linear interpolation, G40: Tool compensation cancel, G64: Cutting mode, G80: Fixed cycle cancel, G94: Per minute feed
When only an axis commanded with G05.1Q2 is commanded. Graphic check is not being carried out. A single block is not being executed.
(2) Command the axis for the spline function mode following G05.1Q2. Note that the command and G05.1Q2. must be in the same block. For example, if the X axis and Y axis are to be commanded in the spline function mode, command «G05.1Q2X0Y0;». The command block containing an axis not designated with this command (G05.1Q2X0Y0) in the spline function mode will carry out linear interpolation instead of spline interpolation.
13. Program Support Functions 13.18 Spline; G05.1
433
(3) If G05.1Q2 is commanded when not in the high-speed high-accuracy control function II mode
(between G05P10000 and G05P0), the program error (P34) will occur. (4) If the machining parameter «#8025 SPLINE ON» is 0 in the high-speed high-accuracy control
function II mode (between G05P10000 and G05P0) and G05.1Q2 is commanded, program error (P34) will occur.
(5) Up to three axes set as the basic axes I, J and K can be commanded for the spline function.
Detailed description
(1) Temporary cancellation of spline interpolation
Normally, once the spline function is activated, one curve is generated by smoothly connecting all points until it is canceled. However, if a corner edge is to be created, or if the segment length is long and spline interpolation is not to be carried out, the function can be canceled temporarily with the parameters. (a) Cancel angle
If the angle of two consecutive blocks exceeds the value set in parameter «#8026 CANCEL ANG.», the spline function will be temporarily canceled, and optimum corner deceleration will be applied. When this parameter is not set (=0), the spline interpolation will be constantly applied. The parameter of the high-accuracy control function «#8020 DCC ANGLE» is valid during the temporary cancellation, and the optimum corner deceleration will be applied.
(Example 1) #8026 CANCEL ANG. = 60
Program command Spline interpolation path
Corner
(Example 2) #8026 CANCEL ANG. = 0
Program commandSpline interpolation path
Curve
13. Program Support Functions 13.18 Spline; G05.1
434
(Note 1) If the section to be a corner is smooth when actual machining is carried out, lower the
CANCEL ANG. If a smooth section becomes a corner, increase the CANCEL ANG. (Note 2) If the CANCEL ANG. DCC. ANGLE, the axis will decelerate at all corners which angle is
larger than the CANCEL ANG. (Note 3) If the CANCEL ANG. < DCC. ANGLE, corner deceleration will not be applied if the corner
angle is less than the DCC. ANGLE even if the spline interpolation is canceled.
(b) Fine segment length
If the movement amount in a block is longer than the parameter «#8030 MINUTE LENGTH», the spline function will be temporarily canceled, and the linear interpolation will be executed. When this parameter is not set (= 0), the fine segment length will be 1mm. If blocks that satisfies the following condition continue, linear interpolation will be executed. Segment length in a block > fine segment length (#8030 MINUTE LENGTH)
Linear interpolation
If the #8030 is set to «-1», the spline interpolation will not be canceled according to the block length.
(c) When a block without movement exists
If a block without movement exists in the spline function, the spline interpolation will be canceled temporarily. Note that blocks containing only «;» will not be viewed as a block without movement.
Block without movement
13. Program Support Functions 13.18 Spline; G05.1
435
(d) When a block markedly longer than other blocks exists in spline function
If the ith block length is Li in the spline interpolation mode, and it is given as «Li > Li — 1 8» or «Li > Li + 1 8», the block will be interpreted as a linear section, and the spline mode will be temporarily canceled. However, if the parameter «#8030 MINUTE LENGTH» is set to «-1», the mode will not be canceled.
«Li > Li — 1 8» or «Li > Li + 1 8»
Li+1 Li-1
(2) Spline interpolation curve shape revision Normally, once the spline function is entered, one curve connecting all points smoothly is generated until the function is canceled. However, if the spline curve shape is to be revised, the spline curve shape can be revised with the parameters. (a) Chord error of block containing inflection point
When changing the CAD curve data into fine segments with the CAM, normally, the tolerance (chord error) of the curve is approximated in segments that are approx. 10m. If there is an inflection point in the curve, the length of the block containing the inflection point may lengthen. (Because the tolerance is applied at both ends near the inflection point.) If the block lengths with this block and the previous and subsequent blocks are unbalanced, the spline curve in this block will have a large error in respect to the original curve. At sections where the tolerance (chord error) of the fine segment block and spline curve in a block containing this type of inflection point, if the chord error in the corresponding section is larger than the value set in parameter (#8027 Toler-1), the spline curve shape is automatically revised so that the error is within the designated value. However, if the maximum chord error of the corresponding section is more than five times larger than the parameter «Toler-1» setting value, the spline function will be temporarily canceled. The curve is revised only in the corresponding block. The revisions are carried out with the following conditions for each block in the spline interpolation mode. There is an inflection point in the spline curve, and the maximum error of the spline curve and linear block is larger than parameter «Toler-1». (Distance between P3-P4 in Fig. 1)
13. Program Support Functions 13.18 Spline; G05.1
436
When the above conditions are satisfied, the spline curve will be revised so that the error between P3-P4 in Fig. 2 is within the designated value.
P0
P1
P2 P3
P4
P5 P6
P7
Spline curve Tolerance (chord error)
Inflection point
Fine segment
Fig. 1 Spline curve before error revision
P4
P3
Spline curve after revision
Spline curve before revision
Chord error designated in the parameter «Toler-1»
Fig. 2 Spline curve after error revision
In parameter «Toler-1», set the tolerance for developing into fine segments with the CAM. Set a smaller value if the expansion (indentation) is apparent due to the relation with the adjacent cutting paths.
(b) Chord error of block not containing inflection point
Even in blocks that do not contain an inflection point, if the block lengths are not matched, the tolerance of the spline curve may increase. The curve may also expand due to the effect of relatively short blocks. At sections where the tolerance (chord error) of the fine segment block and spline curve in a block not containing an inflection point, if the chord error in the corresponding section is larger than the value set in parameter (#8028 Toler-2), the spline curve shape is automatically revised so that the error is within the designated value. However, if the maximum chord error of the corresponding section is more than five times larger than the parameter «Toler-2» setting value, the spline function will be temporarily canceled. The curve is revised only in the corresponding block. The revisions are carried out with the following conditions for each block in the spline interpolation mode. There is no inflection point in the spline curve, and the maximum error of the spline curve and linear block is larger than parameter «Toler-2». (Distance between P2-P3 in Fig. 3)
13. Program Support Functions 13.18 Spline; G05.1
437
When the above conditions are satisfied, the spline curve will be revised so that the error between P2-P3 in Fig. 4 is within the designated value.
P1
P2 P3
P4
P5
Spline curve
Tolerance (chord error) Fine segment
Fig. 3 Spline curve before error revision
P1
P2 P3
P4
P5
Spline curve after revision
Spline curve before revision
Chord error designation parameter «Toler-2»
Fig. 4 Spline curve after error revision
In parameter «Toler-2», set the tolerance for developing into fine segments with the CAM.
(3) Curvature speed clamp The commanded speed F for the spline function during a segment linear arc will be the speed commanded in the previously set modal. However, if the axis is fed with the same speed, excessive acceleration may occur at the sections where the curvature is large (where curvature radius is small) as shown below. Thus, the speed clamp will be applied.
F
F
Curvature small
Acceleration small
Acceleration large
Curvature large
F: Commanded speed (mm/min)
Acceleration and curvature
13. Program Support Functions 13.18 Spline; G05.1
438
With the spline function, the high-accuracy control function is always valid. Thus, even if the curvature changes such as in this curve, the speed will be clamped so that the tolerable value of acceleration/deceleration before interpolation, which is calculated with the parameters, is not exceeded. The clamp speed is set for each block, and the smaller of the curvature radius Rs at the curve block start point and the curvature radius Re at the end point of the block will be used as the main curvature radius R. Using this main curvature radius R, the clamp speed F’ will be calculated with expression (1). The smaller of this clamp speed F’ and the commanded speed F will be incorporated for the actual feedrate. This allows cutting with an adequate feedrate corresponding the curvature radius along the entire curve.
Re
Rs
F’
F’ = R V 60 1000 100 — Ks 100
………………… (1)
V = G1bF (mm/min) G1btL (ms)
G1bF : Target acceleration/deceleration before interpolation
G1btL : Acceleration/deceleration time to reach the target speed
Ks : #8019 R COMP (Accuracy coefficient)
Precautions
(1) The spline function will be canceled during graphic check. (2) This function is valid when the base specifications parameters «#1267 ext03/bit0» is set to «1».
If G05.1 Q2 is commanded when «0» is set, program error (P34) will occur. (3) If the specifications for this function are not provided and G05.1Q2 is commanded, the
program error (P39) will occur. (4) Even if «-1» is set for parameter «#8030 MINUTE LENGTH», the spline function will be
temporarily canceled by the cancel conditions (cancel angle, non-movement block, excessive chord error, etc.) other than the block length.
(5) Command the G05.1 Q2 and G05.1 Q0 commands in independent blocks. A program error (P33) will occur if these are not commanded in independent blocks.
(6) A program error (P33) will occur if the G05.1 command block does not contain a Q command. (7) A program error (P34) will occur if the number of axis in part system does not exceed 3.
Rs : Block start point curvature radius (mm) Re : Block end point curvature radius (mm) R : Block main curvature radius (mm) (smaller one of
Rs and Re) V : Tolerable value of acceleration/deceleration
before interpolation F’ : Clamp speed (mm/min)
13. Program Support Functions 13.19 High-accuracy Spline Interpolation ; G61.2
439
13.19 High-accuracy Spline Interpolation ; G61.2
Function and purpose
This function automatically generates a spline curve that passes through a sequence of points commanded by the fine segment machining program, and interpolates the path along this curve. This allows highly accurate machining at a high speed. This function has two functions; fairing function to delete unnecessary fine blocks, and spline interpolation to connect smoothly a sequence of points commanded by the program. The high-accuracy control function G61.1 is valid also.
Function Contents Fairing Super-fine blocks often included in the data generated with CAM are
deleted. Such a super-fine block scratches the machining surface, and might increase machining time because of acceleration/deceleration. This function avoids these troubles.
Spline interpolation The spline interpolation connects smoothly a sequence of points commanded by program. As a result, the glossy machining surface can be obtained, and the machining time can be reduced because the frequency of the corner deceleration decreases compared with conventional linear interpolation.
Command format
G61.2 X__ Y__ Z__ F__ ;
or
G61.2 ;
G61.2 X Y Z F
: High-accuracy spline interpolation mode ON : X axis end point coordinates : Y axis end point coordinates : ZX axis end point coordinates : Feedrate command
G64 ;
G64 : High-accuracy spline interpolation mode OFF
Detailed description
(1) Fairing
Refer to «Additional functions when high-speed high-accuracy control 2 mode is ON» in «13.17.1 High-speed high-accuracy control».
(2) Spline interpolation Refer to «Detailed description» in «13.18 Spline».
13. Program Support Functions 13.19 High-accuracy Spline Interpolation ; G61.2
440
Example of program
: G91 ; G61.2 ; ………………………………. High-accuracy spline interpolation mode ON G01 X0.1 Z0.1 F1000 ; X0.1 Z-0.2 ; Y0.1 ; X-0.1 Z-0.05 ; X-0.1 Z-0.3 ; G64 ; …………………………………. High-accuracy spline interpolation mode OFF :
(1) The spline function carries out spline interpolation when the following conditions are all
satisfied. If the following conditions are not satisfied, the spline function is canceled once, and it is judged whether to carry out new spline from the next block. It is the movement only of three axes set to the basic axes I, J and K. When the block length is shorter than the machining parameter «#8030 MINUTE LENGTH». When the movement amount is not 0. The group 1 command is G01 (linear interpolation). It is not during the fixed cycle modal. It is not during hypothetical axis interpolation mode. It is not during 3-dimensional coordinate conversion modal. A single block is not being executed.
(2) The spline function is modal command of group 13. This function is valid from G61.2 command block.
(3) The spline function is canceled by group 13 command (G61 to G64). (4) The spline function is canceled by NC reset 2, reset & rewind, NC reset 1 (the setting which
does not hold modal when NC is reset) or power ON/OFF.
Precautions
(1) This function is valid when the base specifications parameters «#1267 ext03/bit0» is set to «1».
If «G61.2» is commanded when «0» is set, program error (P34) will occur. (2) If the specifications for this function are not provided and «G61.2» is commanded, the program
error (P39) will occur. (3) Even if «-1» is set for parameter «#8030 MINUTE LENGTH», the spline function will be
temporarily canceled by the cancel conditions (cancel angle, non-movement block, excessive chord error, etc.) other than the block length.
(4) Graphic check draws a shape of spline interpolation OFF. (5) A program error (P34) will occur if the number of axis in part system does not exceed 3.
13. Program Support Functions 13.20 Scaling ; G50/G51
441
13.20 Scaling ; G50/G51
Function and purpose
By multiplying the moving axis command values within the range specified under this command by the factor, the shape commanded by the program can be enlarged or reduced to the desired size.
Command format
(1) Scaling ON
G51 X__ Y__ Z__ P__ ; Scaling ON X, Y, Z : Scaling center coordinates P : Scaling factor
(2) Scaling cancel
G50 ; Scaling cancel
x1
y1 Y
sc s1 p1
s2 s3
p2 p3
X
sc : Scaling center p1, p2, p3 : Program shape s1, s2, s3 : Shape after scaling
(3) When individually set the scaling factor to three basic axes
G51 X__ Y__ Z__ I__ J__ K__ ; Scaling ON X, Y, Z : Scaling center coordinates I : Scaling factor of basic 1st axis J : Scaling factor of basic 2nd axis K : Scaling factor of basic 3rd axis
13. Program Support Functions 13.20 Scaling ; G50/G51
442
Detailed description
(1) Specifying the scaling axis, scaling center and its factor
Commanding G51 selects the scaling mode. The G51 command only specifies the scaling axis, its center and factor, and does not move the axis. Though the scaling mode is selected by the G51 command, the axis actually valid for scaling is the axis where the scaling center has been specified.
(a) Scaling center
Specify the scaling center in accordance with the then absolute/incremental mode (G90/G91).
The scaling center must be specified also when the current position is defined as a center.
As described above, the axis valid for scaling is only the axis whose center has been specified.
(b) Scaling factor
Use the address P or I, J, K to specify the scaling factor. Minimum command unit : 0.000001 Command range: Either -99999999 to 99999999 (-99.999999 to 99.999999 times) or
-99.999999 to 99.999999 is valid, but the decimal point command is valid only after the G51 command.
When the factor is not specified in the same block as G51, the factor set with the parameter (#8072 SCALING P) is used.
When the address P and the address I, J, K are commanded in the same block, a magnification specified by the address I, J, K is applied for the basic three axes. And a magnification specified by the address P is applied for other axes.
If changed during the scaling mode, the value of this parameter is not made valid. Scaling is performed with the setting value that was used when G51 was commanded.
When the factor is not specified in both the program and parameter, it is calculated as 1.
(c) A program error will occur in either of the following cases. Scaling was commanded though there was no scaling specification. (Program error
(P350)) The upper limit of the factor specifying range was exceeded in the same block as G51.
(Program error (P 35)) (If the machining parameter scaling factor is used, the magnification is calculated as one time in the following cases; -0.000001 <0.000001, more than 99.999999, or less than -99.999999. )
(2) Scaling cancel
When G50 is commanded, scaling is canceled.
13. Program Support Functions 13.20 Scaling ; G50/G51
443
Precautions
(1) Scaling is not applied to the compensation amounts of tool radius compensation, tool position
compensation, tool length compensation and the like. (Compensation is calculated for the shape after scaling.)
(2) Scaling is valid for only the movement command in automatic operation. It is invalid for manual movement.
(3) For X, Y and Z, scaling is valid for only the specified axes and is not applied to the axes not specified.
(4) When an arc is commanded and scaling is valid for one of the two axes configuring the arc plane, a program error (P70) will occur.
(5) When M02 or M30 is commanded, or when NC reset is carried out during the scaling mode, the mode switches to a cancel mode.
(6) When the coordinate system is shifted (G92, G52 command) during scaling, the scaling center is also shifted by the difference amount.
(7) If manual interruption is made during scaling, manual ABS selection is ignored for the movement followed by an incremental value command and operation performed is the same as in manual ABS OFF.
13. Program Support Functions 13.20 Scaling ; G50/G51
444
Example of program
(Example 1)
-50. -100.-150.-200.
-50.
-100.
-150.
N06
N07
N08
N09 N03 N11
Scaling center
D01=25.000
Tool path after 1/2 scaling
Program path after 1/2 scaling
Tool path when scaling is not applied
Program path when scaling is not applied
Y
X
N01 G92 X0 Y0 Z0; N02 G90 G51 X-100. Y-100. P0.5; N03 G00 G43 Z-200. H02; N04 G41 X-50. Y-50. D01; N05 G01 Z-250. F1000; N06 Y-150. F200; N07 X-150.; N08 G02 Y-50. J50.; N09 G01 X-50.; N10 G00 G49 Z0; N11 G40 G50 X0 Y0; N12 M02;
13. Program Support Functions 13.20 Scaling ; G50/G51
445
Relation with other functions
(1) G27 reference position check command When G27 is commanded during scaling, scaling is canceled at completion of the command. (2) Reference position return command (G28, G29, G30) When the G28 or G30 reference position return command is issued during scaling, scaling is
canceled at the midpoint and the axis returns to the reference position. When the midpoint is to be ignored, the axis returns to the reference position directly. When G29 is commanded during scaling, scaling is applied to the movement after the midpoint.
(3) G60 (unidirectional positioning) command If the G60 (unidirectional positioning) command is given during scaling, scaling is applied to
the final positioning point and is not applied to the creep amount. Namely, the creep amount is uniform regardless of scaling.
(4) Workpiece coordinate system switching When the workpiece coordinate system is switched during scaling, the scaling center is shifted
by the difference between the offset amounts of the new and old workpiece coordinate systems.
(5) During figure rotation When scaling is commanded during figure rotation, scaling is applied to the center of the figure
rotation and the rotating radius. (6) Scaling command in figure rotation subprogram When scaling is commanded in the subprogram of the figure rotation, scaling can be applied
only to the shape designated by the subprogram without applying scaling to the rotating radius of the figure rotation.
(7) During coordinate rotation When scaling is commanded during coordinate rotation, the scaling center rotates. Scaling is
executed at that rotated scaling center. (8) G51 command When the G51 command is issued during the scaling mode, the axis whose center was newly
specified is also made valid for scaling. Also, the factor under the latest G51 command is made valid.
13. Program Support Functions 13.21 Coordinate Rotation by Program ; G68/G69
446
13.21 Coordinate Rotation by Program; G68/G69
Function and purpose
When machining a complicated shape at a position rotated in respect to the coordinate system, the shape before rotation can be programmed on the local coordinate system, rotation angle designated with the program coordinate rotation command, and the rotated shaped machined.
Command format
(1) Coordinate rotation ON
G68 X__ Y__ R__; Coordinate rotation ON G68 : Coordinate rotation command X, Y : Rotation center coordinates.
Two axes (X,Y or Z) corresponding to the selected plane are designated with absolute positions.
R : Rotation angle The counterclockwise direction is +.
Select the command plane with G17 to G19.
(2) Coordinate rotation cancel
G69 ; Coordinate rotation cancel
r1(Rotation angle) (x1,y1) (Rotation center)
W (Original local coordinate)
W’ (Rotated local coordinate system)
x1
X’
X
Y’
Y
y1
13. Program Support Functions 13.21 Coordinate Rotation by Program ; G68/G69
447
Detailed description
(1) Always command the rotation center coordinate (x1, y1) with an absolute value. Even if
commanded with an incremental address, it will not be handled as an incremental value. The rotation angle «r» depends on the G90/G91 modal.
(2) If the rotation center coordinates (x1, y1) are omitted, the position where the G68 command was executed will be the rotation center.
(3) The rotation takes place in the counterclockwise direction by the angle designated in rotation angle r1.
(4) The rotation angle r1 setting range is -360.000 to 360.000. If a command exceeding 360 degrees is issued, the remainder divided by 360 degrees will be the command.
(5) Since the rotation angle «r1» is modal data, if once commanded, it will not be changed until the new angle data is commanded. Thus, the rotation angle «r1″can be omitted. If the rotation angle is omitted in spite that G68 is commanded for the first time, «r1» will be regarded as 0.
(6) The program coordinate rotation is a function used on the local coordinate system. The relation of the rotated coordinate system, workpiece coordinate system and basic machine coordinate system is shown below.
(6) The coordinate rotation command during coordinate rotation is processed as center
coordinates and rotation angle changes. (7) If M02 or M30 is commanded or the reset signal is input during the coordinate rotation mode,
the coordinate rotation mode will be canceled. (8) G68 is displayed on the modal information screen during the coordinate rotation mode. When
the mode is canceled, the display changes to G69. (The modal value is not displayed for the rotation angle command R.)
(9) The program coordinate rotation function is valid only in the automatic operation mode.
Basic machine coordinate system
Workpiece coordinate system
Local coordinate system (x1,y1)=(0,0)
Rotation angle (R)
13. Program Support Functions 13.21 Coordinate Rotation by Program ; G68/G69
448
Example of program (Program coordinate rotation by absolute command)
N01 G28 X0. Y0.; N02 G54 G52 X200. Y100. ; Local coordinate designation N03 T10 ; N04 G68 X-100. Y0. R60. ; Coordinate rotation ON N05 M98 H101 ; Subprogram execution N06 G69 ; Coordinate rotation cancel N07 G54 G52 X0 Y0 ; Local coordinate system cancel N08 M02 ; End Subprogram (Shape programmed with original coordinate system) N101 G00 X-100. Y-40.; N102 G83 X-150. R-20. F100 ; N103 G00 Y40. ; N104 G83 X-150. R-20. F100 ; N105 M99
-100.
Actual machining shape
(Programmed coordinates) -100.
100.
Y
X
100. 200. -100. N101
N102
N103
N104
Y’ X’
60
Local coordinates (before rotation)
13. Program Support Functions 13.21 Coordinate Rotation by Program ; G68/G69
449
Example of program (Operation of only one axis was commanded by first movement command after coordinate rotation command)
Command basically two axes in the rotation plane by the absolute value immediately after the coordinate rotation command. When commanding one axis only, the following two kinds of operation can be selected by the parameter «#19003 PRG coord rot type».
(1) When «#19003 PRG coord rot type» is «1», the operation is the same as that with «G50.Y0.» commanded in N04. The end point is calculated on the assumption that the start point rotates along with the coordinates’ rotation.
N01 G17 G28 X0. Y0.; N02 G90 G92 G53 X0. Y0.; N03 G68 X40. Y0. R90.; Coordinate rotation ON N04 X50.; N05 Y50.; N06 G69 ; Coordinate rotation cancel N07 M02 ; End
(Local coordinate system before
rotation)
(Local coordinate system after rotation)
N04
Y
X
X’
Y’
N05
(Rotation center) X=-10
Y=10
Machine movement path
(The start point is rotated virtually.)
(X’,Y’)=(50,50)
Start point: (X,Y)=(0,0)
X=50
Y=50
(X’,Y’)=(40,40)
(2) When «#19003 PRG coord rot type» is «0», only axis commanded in N04 (X’ Axis) is moved.
The start point does not rotate along with the coordinate rotation; therefore the end position is calculated based on the current position on local coordinate system before rotation.
N04
Y
X
X’
Y’
N05
(Rotation center) X=-10
Y=10
Machine movement path
X’=50
Y’=50
Start point: (X,Y)=(40,40)
N01 G17 G28 X0. Y0.; N02 G90 G92 G53 X0. Y0.; N03 G68 X40. Y0. R90.; Coordinate rotation ON N04 X50.; N05 Y50.; N06 G69 ; Coordinate rotation cancel N07 M02 ; End
(Local coordinate system after rotation)
(X’,Y’)=(0,0)
(Local coordinate system before rotation)
(X’,Y’)=(50,50)
13. Program Support Functions 13.21 Coordinate Rotation by Program ; G68/G69
450
Example of program (Local coordinate designation during program coordinate rotation)
(1) When «#19003 PRG coord rot type» is «0», it is on the coordinate system after coordinates
rotation that the commanded position is set as the local coordinate zero point. (2) When «#19003 PRG coord rot type» is «1», it is on the coordinate system before coordinates
rotation that the commanded position is set as the local coordinate zero point. Then the coordinates system is rotated.
N01 G17 G28 X0. Y0.; N02 G90 G92 G53 X0. Y0.; N03 G68 X20. Y0. R90.; Coordinate rotation ON N04 G52 X10. Y10.; Local coordinate designation N05 X20.; N06 Y10.; N07 G69 ; Coordinate rotation cancel N08 M02 ; End
N03
(Local coordinate system)
Y
X
Y’
(Rotation center) (Workpiece coordinate system)
(1) Operation of #19003 = 0 (2) Operation of #19003 = 1
Y,Y’
X,X’ (Workpiece coordinate system)
N04
Y
X
Y’
Y»
(Workpiece coordinate system)
Y,Y’
X,X’
X»
Y»
(Rotation center) (Workpiece coordinate system)
(Local coordinate designation)
N05
Y
X
X»
Y»
(Workpiece coordinate system)
Y
X
X»
Y»
(Rotation center)
(Workpiece coordinate system)
(The start point is rotated virtually.)
N06
Y
X
X»
Y»
(Workpiece coordinate system)
Y
X
X»
Y»
(Workpiece coordinate system)
(Local coordinate system)
Start point: (X»,Y»)=(10,30)
(X»,Y»)=(20,30)
(Local coordinate system)
(Local coordinate system)
Start point: (X»,Y»)=(-10,-10)
(X»,Y»)=(20,-10)
(X»,Y»)=(20,30) (X»,Y»)=(20,10)
(X»,Y»)=(10,30)
(X»,Y»)=(20,-10)
(X»,Y»)=(20,10)
(Local coordinate system)
Y=-20
X=20
X=30
Y=-10
X=30
Y=-10
Y=1 Y=1
X=40
Y=1
X=30
Y=10
X=40 X=20
W
X’
W’
Workpiece coordinate system is rotated virtually. Workpiece coordinate system is not rotated.
W,W’ (Workpiece coordinate system after rotation)
X’ X»
The workpiece coordinate zero point after rotation is considered as
(X,Y)=(0,0). The position after shifted by 10 each in the X and Y
direction is set as the local coordinate zero point.
— The direction of the shift is not the direction of X’ and Y’.
Designate the local coordinate system on the workpiece coordinate system.
The commanded axis moves on the rotation coordinate system. — Axis without movement command does not move.
The commanded axis moves on the rotation coordinate system. — Axis without movement command moves to the position on
rotation coordinate system.
W,W’
(Local coordinate designation)
(Workpiece coordinate system is rotated virtually.)
W
L
L L
L L
W
W
W
W
L
(Local coordinate system)
(X,Y)=(10,10) (X,Y)=(0,0)
13. Program Support Functions 13.21 Coordinate Rotation by Program ; G68/G69
451
Example of program (Coordinate system designation during program coordinate rotation)
When the coordinate system setting (G92) is executed during program coordinate rotation, this program operates similarly as «Local coordinate designation during program coordinate rotation».
(1) When «#19003 PRG coord rot type» is «0», it is on the coordinate system after coordinates rotation that the current position is preset to the command position. (Ex.) Setting on the coordinate system (X’-Y’) after coordinate rotation
G54(0, 0) X
Y
X’
Y’
10.
10.
G68 X0 Y0 R30. G0 X10. Y10. G92 X0. Y0.
G54(0, 0) X
Y
X’
Y’
10. 10.
G92 shift amount
Command position
Position after rotation
(2) When «#19003 PRG coord rot type» is «1», it is on the coordinate system before coordinates
rotation that the current position is preset to the command position. Then the coordinate system is rotated. (Ex.) Setting on the coordinate system (X-Y) after coordinate rotation
G54(0, 0) X
Y
X’
Y’
10.
10.
G68 X0 Y0 R30. G0 X10. Y10. G92 X0. Y0.
G54(0, 0) X
Y
X’
Y’
10.
10. G92 shift amount
Command position
Position after rotation
(Note 1) When «#19003 PRG coord rot type» is «1» and the coordinate system setting (G92) is
executed during coordinate rotation mode, the rotation center of program coordinate rotation is not shifted. (The same position from the basic machine coordinate system)
13. Program Support Functions 13.21 Coordinate Rotation by Program ; G68/G69
452
Precautions
(1) Always command an absolute value for the movement command immediately after G68 and
G69. (2) If manual absolute is ON and manual interrupt is issued for the coordinate rotation axis, do not
use automatic operation for the following absolute value command. (3) The intermediate point during reference position return is the position after the coordinates are
rotated. (4) If the workpiece coordinate system offset amount is changed during the coordinate rotation
mode, the rotation center for the program coordinate rotation will be shifted. (The center will follow the coordinate system.)
(5) If the workpiece coordinates are changed during the coordinate rotation mode (ex., from G54 to G55), the rotation center of the program coordinate rotation will be the position in the commanded coordinate system. (The center position will be the same looking from the basic machine coordinate system.)
(6) If coordinate rotation is executed to the G00 command for only one axis, two axes will move. If G00 non-interpolation (parameter «#1086 G0Intp» = 1) is set, each axis will move independently at the respective rapid traverse rates. If the axis must be moved linearly (interpolated) from the start point to the end point (such as during the hole machining cycle), always turn G00 non-interpolation OFF (parameter «#1086 GOIntp» = 0). The feedrate in this case is the composite speed of each axis’ rapid traverse rate, so the movement speed will be faster than when moving only one axis (before coordinate rotation).
(7) If the coordinate rotation specifications are not provided, a program error (P260) will occur when coordinate rotation is commanded.
(8) The offset operation during the coordinate rotation mode compensates the local coordinate system after coordinate rotation. The compensation direction is the coordinate system before rotation.
(9) Mirror image during the coordinate rotation mode is applied on the local coordinate system after coordinate rotation.
(10) All position displays show the positions after coordinate rotation with the local coordinate system before rotation.
(11) When the coordinate value variables are read, the positions are all on the coordinate system before rotation.
(12) The coordinates can also be rotated for the parallel axis. Select the plane that contains the parallel axis before issuing the G68 command. The plane cannot be selected in the same block as the G68 command.
(13) The coordinates can be rotated for the rotation axis. The angle will be interpreted as a length when rotating.
Relation with other functions
(1) Program error (P111) will occur if the plane selection code is commanded during the
coordinate rotation mode. (2) Program error (P485) will occur if pole coordinate interpolation is commanded during the
coordinate rotation mode. (3) Program error (P481) will occur if coordinate rotation is commanded during the pole
coordinate interpolation mode. (4) Program error (P485) will occur if cylindrical interpolation is commanded during the coordinate
rotation mode. (5) Program error (P481) will occur if coordinate rotation is commanded during the cylindrical
interpolation mode. (6) Program error (P34) will occur if the workpiece coordinate system preset (G92.1) is
commanded during the coordinate rotation mode. (7) Program error (P34) will occur if high-accuracy control mode, high-speed machining mode 3,
high-speed high-accuracy I or II is commanded during the coordinate rotation mode.
13. Program Support Functions 13.22 Coordinate Rotation Input by Parameter; G10
453
13.22 Coordinate Rotation Input by Parameter; G10
Function and purpose
If a deviation occurs between the workpiece alignment line and machine coordinate system’s coordinate axis when the workpiece is mounted, the machine can be controlled to rotate the machining program coordinates according to the workpiece alignment line deviation. The coordinate rotation amount is set with the parameters. The parameter can be set on the parameter setting screen or with the G10 command. Note that when the G10 command is used, the separate additional specification «parameter input by program» is required. The following is in the case where G10 command is issued.
Ym
Xm
G56
G54
G55
G57
W1′
W2′
W3′
W4′
Rotation center
Rotation angle
M Basic machine coordinates
W1
W2
13. Program Support Functions 13.22 Coordinate Rotation Input by Parameter; G10
454
Command format
G10 I__ J__ ;
G10 K__;
I : Horizontal vector. Command a value corresponding to Coord rot plane (H) which is set in the parameter input screen. Command range: -999999.999999 to 999999.999999 Coordinate rotation angle is automatically calculated when commanding vector contents.
J : Vertical vector. Command a value corresponding to Coord rot plane (V) which is set in the parameter input screen. Command range: -999999.999999 to 999999.999999 Coordinate rotation angle is automatically calculated when commanding vector contents.
K : Rotation angle. Command a value corresponding to Coord rot angle which is set in the parameter input screen. Command range: -360.000000 to 360.000000 Set the vector contents to 0 when commanding coordinate rotation angle.
Parameters specified in the parameter setting screen can be changed from the machining program.
Detailed description
(1) As for the rotation center coordinate position, designate the position on the machine
coordinate system. (2) All workpiece coordinate systems from G54 to G59 rotate with the rotation command.
While the machine coordinate system does not rotate, it can be understood that there is a hypothetical machine coordinate system in the coordinate system after rotation.
(3) The coordinate value counter does not rotate. The position in the original workpiece coordinate system (non-rotated) is displayed.
(4) If the setting is made on the parameter setting screen, the setting is validated with the cycle start after the parameter is set. If set with the G10 command, settings are immediately validated.
13. Program Support Functions 13.22 Coordinate Rotation Input by Parameter; G10
455
Example of program
(1) To use for compensating positional deviation of pallet changer
Y
X M
+
+
+
+ G56
G57
G54
G55
Rotation movement (15 degree)
N01 G28 X0 Y0 Z0 ; N02 M98 P9000 ; Pallet deviation measurement N03 G90 G53 X0 Y0 ; Parallel movement amount shift N04 G92 X0 Y0 ; Parallel movement amount definition N05 G10 K15. ; Rotation amount definition N06 G90 G54 G00 X0 Y0 ; G54 workpiece machining N07 M98 H101 ; N08 G90 G55 G00 X0 Y0 ; G55 workpiece machining N09 M98 H101 ; N10 G90 G56 G00 X0 Y0 ; G56 workpiece machining N11 M98 H101 ;
N12 G90 G57 G00 X0 Y0 ; G57 workpiece machining N13 M98 H101 ; N14 G27 X0 Y0 Z0 ; N15 M02 ; Machining shape program N101 G91 G01 G42 D01 F300 ; N102 X100 ; N103 G03 Y50. R25. ; N104 G01 X-100. ; N105 G03 Y-50. R25. ; N106 G01 G40 ; N107 M99 ;
Precautions
(1) If rotation angle zero is commanded while carrying out coordinate rotation, it will be canceled
at the next movement command regardless of the G90 or G91 setting. (2) Command the first movement after this command with the G00 or G01 mode. If an arc
command is issued, the arc start point will not be rotated. However, only the arc end point will rotate. This will cause the start point radius and end point radius to differ, and the program error (P70) will occur.
(3) When data is input with the data input/output function, coordinate rotation angle is considered to exist, and automatic calculation from the vector component will not be executed.
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
456
13.23 3-dimensional Coordinate Conversion ; G68/69
Function and purpose
With the 3-dimensional coordinate conversion function, a new coordinate system can be defined by rotating and moving in parallel the zero point in respect to the X, Y and Z axes of the currently set workpiece coordinate system. By using this function, an arbitrary spatial plane can be defined, and machining on that plane can be carried out with normal program commands. An option is required to validate this function. If the 3-dimensional coordinate conversion is commanded when the option is not added, a program error will occur.
Y’
X’ Machine coordinate system
X
Y
Workpiece coordinate system
G68 program coordinate system
Z’
Z
When the G68 command is issued, the zero point is shifted by the command value (x, y, z) in respect to the current local coordinate system. A new G68 program coordinate system rotated by the designated rotation angle «r» in respect to the commanded rotation center direction (i, j, k) is created. The local coordinate system is the same as the workpiece coordinate system when the local coordinate system offset is not ON.
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
457
Command format
G68 X__ Y__ Z__ I__ J__ K__ R__ ;
G68 : 3-dimensional coordinate conversion mode command X,Y,Z : Rotation center coordinates
Designate with the absolute position of the local coordinate system. I,J,K : Rotation center axis direction (1: Designated 0: Not designated)
Note that «1» is designated for only one of the three axes. «0» is designated for the other two axes.
R : Rotation angle The counterclockwise direction looking at the rotation center from the rotation center axis direction is positive (+). The setting range is -360 to 360, and the increment follows the setting and display unit.
G69 ;
G69 : 3-dimensional coordinate conversion mode cancel command
Detailed description
(1) Command the rotation center coordinates with absolute values. (2) If the rotation center coordinates are omitted, the zero point of the currently set coordinate
system will be the rotation center coordinates. (3) Designate values for I, J and K. If even one is not designated, program coordinate rotation
command will be valid. (4) Set «1» in only one of I, J and K, and set «0» for the other two.
The program error (P33) will occur if «1» is set in two or more. (5) The program error (P33) will also occur if «0» is set for all I, J and K. (6) When addresses I, J and K are not designated, this will be handled as the program coordinate
rotation. (7) If a number other than «0» (including two-digit numbers) is designated for addresses I, J and K,
this will be handled as «1». If a blank is designated, this will be handled as «0». (8) If a G code that cannot be commanded in the 3-dimensional coordinate conversion modal is
issued, the program error (P921) will occur. When the 3-dimensional coordinate conversion is commanded during the modal where 3-dimensional coordinate conversion cannot be carried out, the program error (P922) will also occur. Furthermore, the G codes that cannot be commanded together with G68 are commanded in the same block as G68, the program error (P923) will occur.
(9) The 3-dimensional coordinate conversion command for the rotary axis will result in the program error (P32).
(10) If a 3-dimensional coordinate conversion command is issued when there is no specifications for 3-dimensional coordinate conversion, the program error (P920) will occur.
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
458
Example of program 1
N1 G68 X10.Y0. Z0. I0 J1 K0 R-30.; N2 G68 X0. Y10. Z0. I1 J0 K0 R45.; ; N3 G69;
+Z +Y
+X
+Z’
+X’
+Z»
+Y»
+Y’ +X»
45
P(0,0,0)
Local coordinate system (workpiece coordinate system)
P'(10,0,0)
G68 program coordinate system (A)
-30
P»(0,10,0) G68 program coordinate system (B)
(1) With N1, the origin is shifted by [x, y, z] = (10., 0, 0) in respect to the currently set local coordinate system. The new G68 program coordinate system (A in the figure above) rotated -30 in the counterclockwise direction using the Y axis as the center is set.
(2) With N2, the origin is shifted by [x, y, z] = (0, 10., 0) in respect to the newly set G68 program coordinate system (A in the figure above). The new G68 program coordinate system (B in the figure above) rotated +45 in the counterclockwise direction using the X axis as the center is set.
(3) With N3, the G68 program coordinate systems that have been set are all canceled, and the state prior to where the first G68 has been commanded is returned.
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
459
Coordinate system
(1) By issuing the 3-dimensional coordinate conversion command, a new coordinate system (G68
program coordinate system) will be created on the local coordinate system. (2) The coordinate system for the 3-dimensional coordinate conversion rotation center
coordinates is the local coordinate system. Thus, these coordinate systems are affected by the following coordinate system offset and coordinate system shift amount. Local coordinate system offset issued with G52 command G92 shift amount issued with G92 command Coordinate system offset corresponding to workpiece coordinate system selected with
command External workpiece coordinate offset Manual interruption amount or manual feed amount when manual ABS is OFF
(3) If 3-dimensional coordinate conversion is commanded again during the 3-dimensional coordinate conversion modal, a G68 program coordinate system is created on the current G68 program coordinate system, and is used as a new G68 program coordinate system.
(4) The local coordinate system cannot be created (G52) on the G68 program coordinate system.
(If G52 is issued, the program error (P921) will occur.) (5) G68 program coordinate system can be reset either by G69 command or reset inputting.
(Exclude reset 1 when «0» is set to the parameter «#1151 rsint».)
Rotation angle
(1) For the rotation angle, the counterclockwise direction looking at the rotation center from the
plus direction of the rotation center axis is the plus (+) direction. (2) The rotation angle command unit with no decimal point depends on the parameter «#1078
Decpt» (Decimal point type 2). (3) If the rotation angle is omitted, the rotation angle will be handled as 0.
Rotation center coordinate
(1) The G68 rotation center coordinate system is commanded with the local coordinate system
(G68 program coordinate system during the 3-dimensional coordinate conversion modal). (2) The rotation center coordinate designation is handled as an absolute value designation
whether or not an absolute/incremental modal (G90/G91) is currently being executed. (3) If the rotation center coordinate is omitted, it will be handled as if the zero point of the current
local coordinate (G68 program coordinate system during the 3-dimensional coordinate conversion modal) is designated for the omitted address’s axis. (The same as when «0» is just set.)
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
460
G68 multiple commands
By commanding 3-dimensional coordinate conversion during the 3-dimensional coordinate conversion modal, two or more multiple commands can be issued.
(1) The 3-dimensional coordinate conversion command in the 3-dimensional coordinate conversion modal is combined with the conversion in the modal.
(2) If the 3-dimensional coordinate conversion is overlapped during the 3-dimensional coordinate conversion modal, the overlapped 3-dimensional coordinate conversion will be created on the coordinate system (G68 program coordinate system) created with the 3-dimensional coordinate conversion in the modal. Thus, the rotary axis and coordinates must be designated with this G68 program coordinate system. If creating a 90 rotated coordinate system for X axis and Y axis each, commands must be issued as in Example 2, but example 1. G68 X0.Y0.Z0.I1J0K0 R90.;
G68 X0.Y0.Z0.I0J1K0 R90.; X axis rotation 90 Y axis rotation 90 (Th (Y axis designated here is the same as the Z axis in the original coordinate system.)
G68 X0.Y0.Z0.I1J0K0 R90.; G68 X0.Y0.Z0.I0J0K1 R-90.;
X axis rotation 90 Z axis rotation 90 (Th (Z axis -90 rotation designated here is the same as the Y axis +90 rotation in the original coordinate system.)
Conversion method for 3-dimentional coordinate conversion
The coordinate values (Xp, Yp, Zp) in the newly set G68 program coordinate system and the coordinate values (Xm, Ym, Zm) in the reference workpiece coordinate system are converted as shown below. First G68 command
[Xm, Ym, Zm, 1] = [Xp, Yp, Zp, 1] R1T1 (Forward row) [Xp, Yp, Zp, 1] = [Xm, Ym, Zm, 1] (T1-1) (R1-1) (Reverse row)
Second G68 command
[Xm, Ym, Zm, 1] = [Xp, Yp, Zp, 1] R2T2R1T1 [Xp, Yp, Zp, 1] = [Xm, Ym, Zm, 1] (T1-1) (R1-1) (T2-1) (R2-1)
R1, R2: Rotation row calculated from first and second G68 parameter T1, T2: Movement row calculated from first and second G68 parameter
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
461
The conversion rows Rn and Tn (n = 1, 2) are as follow. Rn conversion row
I designation (rotation around X axis)
J designation (rotation around Y axis)
K designation (rotation around Z axis)
1 0 0 0
0 cosR sinR 0
0 -sinR cosR 0
0 0 0 1
cosR 0 -sinR 0
0 1 0 0
sinR 0 cosR 0
0 0 0 1
cosR sinR 0 0
-sinR cosR 0 0
0 0 1 0
0 0 0 1
Tn conversion row
1 0 0 0
0 1 0 0
0 0 1 0
x y z 1
x, y, z I, J, K R
: Rotation center coordinates (parallel movement amount) : Rotation axis selection : Rotation angle
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
462
Precautions related to arc command
If the first command after the 3-dimensional coordinate conversion command was an arc shape, and the center of the arc did not change before and after the 3-dimensional coordinate conversion, an arc is drawn. However, an error will occur in the following cases:
(1) For the arc in which the arc center is specified with I and J, if the center coordinate has been
deviated followed by the 3-dimensional coordinate conversion, a program error (P70 Major arc end position deviation) will occur.
Current position
Y
X End point (X 100, Y 0) Arc center
(X 50, Y 0)
Y Y’
(X 100, Y 0)
Arc center (X’ 50, Y’ 0)
End point
(X’ 100, Y’ 0) X X’
Program error
Example in which program error (P70) occurs
G90 G28 X0 Y0 Z0 ; F3000 G17 ; G68 X100. Y0. Z0. I0 J0 K1 R0. ; G02 X100. I50. ;
No 3-dimensional coordinate conversion In 3-dimensional coordinate conversion
Current position
(2) For the arc in which the arc radius is specified with R, If the center coordinate has been deviated
followed by the 3-dimensional coordinate conversion, a program error (P71 Arc center calculation disabled) will occur.
Y
X End point (X 100, Y 0)
Y Y’
(X 100, Y 0) End point (X’ 100, Y’ 0)
X X’
Program error
Example in which program error (P71) occurs
G90 G28 X0 Y0 Z0 ; F3000 G17 ; G68 X100. Y0. Z0. I0 J0 K1 R0. ; G02 X100. R50. ;
No 3-dimensional coordinate conversion In 3-dimensional coordinate conversion
Radius = 50 Radius50
Current position
Current position
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
463
Example of program 2
This is a sample program only to explain about the operations. (To actually proceed with the machining by using this program, the dedicated tools and the tool change functions are required.)
(1) Example of machining program using arc cutting
In the following program example, the arc cutting (N3 block) carried out on the top of the workpiece is also carried out on the side of the workpiece. By using 3-dimensional coordinate conversion, the side can be cut with the same process (N8 block).
N01 G17 G90 G00 X0 Y0 Z0; Position to the workpiece zero point P. N02 G00 X100. Y200. Z200.; Move to (100, 200, 200) with rapid traverse. N03 G02 X100. Y400. J100. F1000;
Carry out arc cutting on workpiece top.
N04 G00 Z300.; Escape in +Z direction at +100 rapid traverse. N05 G68 X0 Y0 Z200. I0 J1 K0 R90.;
After shifting program coordinate system to (0, 0, 200), rotate coordinate axis +90 in Y axis direction. Set the program coordinate system (X’ Y’ Z’) which has been rotated +90in the Y axis direction around the (0,0,200).
N06 G17 G90 G00 X0 Y0 Z0; Position to the new program zero point P’. N07 G00 X100. Y200. Z200.; Move to G68 program coordinate system (100, 200, 200) and
workpiece coordinate system (200, 200, 100) with rapid traverse.
N08 G02 X100. Y400. J100. F1000;
Carry out arc cutting on workpiece side.
N09 G00 Z300.; Move +100 in program coordinate system + Z’ direction with rapid traverse.
N10 G69; N11 M02;
+X’
+X
N1
P (0,0,0)
N2
N3
N4
N6
P’ (0,0,200)
+Z
+Z’
N7 N9
+Y’
+Y
N8
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
464
(2) Example of machining program using fixed cycle
In the following program, the bolt hole cycle (N08 block) executed on the top of the workpiece is also carried out on the side of the workpiece. By using 3-dimensional coordinate conversion, the side can be cut with the same process (N18 block).
N01 G90 G00 X0 Y0 Z0; Position to the workpiece coordinate system’s 1st
workpiece zero point. N02 F2000; N03 G00 X100. Y100. Z-600.; Move to (100, 100, -600) with rapid traverse. N04 G52 X100. Y100. Z-600.; Set the local coordinate system to the (100, 100, -600)
position. N05 G00 X100. Y10. Z 200.; Move to the local coordinate system (X’,Y’,Z’)’s (100, 10,
200) position with rapid traverse. N06 G91; Incremental value command N07 G81 Z-10. R5. L0 F2000; Drilling N08 G34 X100. Y200. I90. J270. K10.; Bolt hole cycle N09 G80; Drilling cancel N10 G91 G00 X-200.; Move -200 from machining end point to X axis direction
with rapid traverse. N11 G90 G52 X0 Y0 Z0; Cancel local coordinate system. N12 G90 G00 X0 Y0 Z0; Position to workpiece zero point. N13 G00 X100. Y100. Z-400.; Move to (100, 100, -400) with rapid traverse. N14 G68 X100. Y100. Z-400. I0 J1 K0 R90.;
Set G68 program coordinate system (X»,Y»,Z») to position rotated +90 in Y axis direction using (100, 100, -400) position as center.
N15 G00 X100.Y10. Z200.; Move to (100, 10, 200) position in G68 program coordinate system with rapid traverse.
N16 G91; Incremental value command N17 G81 Z-10. R5. L0 F200; Drilling N18 G34 X100.Y200. I90. J270. K10.; Bolt hole cycle N19 G80; Drilling cancel N20 G91 G00 X-200.; Move -200 from machining end point to X axis direction
with rapid traverse. N21 G69; Cancel 3-dimensional coordinate conversion modal. N22 M02; End program.
-Z
O (0,0,0)
N1
+ Y
+ X
N3
+Z’
O’ (100,100,-600)
+X»
N5
N10
N12
N13
O» (100,100,-400)
N15
N20
N7~N9
N17~N19
+Y»
+X’
+Z»
+Y
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
465
Relation with other functions (Relation with other G codes)
Pxxx in the list indicates the program error Nos.
Format Function
When this command is designated during
3-dimensional coordinate conversions
When 3-dimensional coordinate conversion is designated in this modal
status
When 3-dimensional coordinate conversion
is designated in the same block
G00 Positioning P923 G01 Linear interpolation P923
Circular interpolation CW
P923 G02
Helical interpolation CW P921 P922 P923 Circular interpolation CW
P923 G03
Helical interpolation CCW
P921 P922 P923
G02.3 Exponential interpolation CW
P921 P922 P923
G02.4 3-dimensional circular interpolation CW
P921 P922 P923
G03.3 Exponential interpolation CCW
P921 P922 P923
G03.4 3-dimensional circular interpolation CCW
P921 P922 P923
G04 Dwell — G04 valid, G68 ignored G05 P0 High-speed machining
mode cancel — P923
G05 P1,2 High-speed machining mode I, II
P34 illegal G code P34 illegal G code P923
G05 P10000 High-speed high-accuracy control II
P34 illegal G code P34 illegal G code P923
G05.1 Q0 High-speed machining mode/High-speed high-accuracy control cancel
P923
G05.1 Q1 High-speed high-accuracy control I
P923
G05.1 Q2 Fine spline P34 illegal G code P34 illegal G code P923 G07.1/G107 Cylindrical interpolation P921 P481 illegal G code (mill) P923 G09 Exact stop check — P923
Parameter input by program
P421 parameter input error P923 G10
Tool compensation data input by program
— G10 valid, G68 ignored
G11 Parameter input by program cancel
— P923
G12 Circle cutting CW — P923 G12.1 Polar coordinate
interpolation P921 P481 illegal G code (mill) P923
G13 Circle cutting CCW — P923 G13.1 Polar coordinate
interpolation cancel — P923
G15 Polar coordinate command cancel
— P923
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
466
Format Function
When this command is designated during
3-dimensional coordinate conversions
When 3-dimensional coordinate conversion is designated in this modal
status
When 3-dimensional coordinate conversion
is designated in the same block
G16 Polar coordinate command
P923
G17 Plane selection X-Y G18 Plane selection Z-X G19 Plane selection Y-Z G20 Inch command G21 Metric command G27 Reference position
check — G27 valid, G68 ignored
G28 Reference position return
— G28 valid, G68 ignored
G29 Start point return — G29 valid, G68 ignored G30 2nd to 4th reference
position return — G30 valid, G68 ignored
G30.1 Tool position return 1 — G30.1 valid, G68 ignored G30.2 Tool position return 2 — G30.2 valid, G68 ignored G30.3 Tool position return 3 — G30.3 valid, G68 ignored G30.4 Tool position return 4 — G30.4 valid, G68 ignored G30.5 Tool position return 5 — G30.5 valid, G68 ignored G30.6 Tool position return 6 — G30.6 valid, G68 ignored G31 Skip — P923 G31.1 Multi-step skip 1 — P923 G31.2 Multi-step skip 2 — P923 G31.3 Multi-step skip 3 — P923 G33 Thread cutting P921 P922 P923 G34 Special fixed cycle
(bolt hole circle) — P923
G35 Special fixed cycle (line at angle)
— P923
G36 Special fixed cycle (arc)
— P923
G37.1 Special fixed cycle (grid)
— P923
G37 Automatic tool length measurement
P921 — G37 valid, G68 ignored
G38 Tool radius compensation (vector designation)
— P923
G39 Tool radius compensation (corner arc)
— P923
G40 Tool radius compensation (cancel)
—
Tool radius compensation
P922 P923 G41
3-dimensional tool radius compensation
P922 P923
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
467
Format Function
When this command is designated during
3-dimensional coordinate conversions
When 3-dimensional coordinate conversion is designated in this modal
status
When 3-dimensional coordinate conversion
is designated in the same block
Tool radius compensation
P922 P923 G42
3-dimensional tool radius compensation
P922 P923
G40.1/G150 Normal line control cancel
P921 — P923
G41.1/G151 Normal line control (left)
P921 P922 P923
G42.1/G152 Normal line control (right)
P921 P922 P923
G43 Tool length compensation (+)
P923
G44 Tool length compensation (-)
P923
G45 Tool position compensation increase
— P923
G46 Tool position compensation decrease
— P923
G47 Tool position compensation 2-fold increase
— P923
G48 Tool position compensation 2-fold decrease
— P923
G49 Tool length compensation cancel
— P923
G43.1 Tool length compensation in tool axis direction
P927 P931 P923
G43.4/G43.5 Tool center point control type 1/2 ON
P941 P922 P923
G50 Scaling cancel P921 — P923 G51 Scaling ON P921 P923 G50.1 Mirror image cancel — P923 G51.1 Mirror image ON P923 G52 Local coordinate system
setting P921 — G52 valid, G68 ignored
G53 Machine coordinate system setting
— G53 valid, G68 ignored
G54 Workpiece coordinate system 1 selection
P921 P923
G55 Workpiece coordinate system 2 selection
P921 P923
G56 Workpiece coordinate system 3 selection
P921 P923
G57 Workpiece coordinate system 4 selection
P921 P923
G58 Workpiece coordinate system 5 selection
P921 P923
G59 Workpiece coordinate system 6 selection
P921 P923
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
468
Format Function
When this command is designated during
3-dimensional coordinate conversions
When 3-dimensional coordinate conversion is designated in this modal
status
When 3-dimensional coordinate conversion
is designated in the same block
G54.1 Extended workpiece coordinate system selection
P921 P923
Unidirectional positioning
P921 — G60 valid, G68 ignored G60
Unidirectional positioning (Modal designation)
P921 P922 P923
G61 Exact stop check mode P923 G61.1 High-accuracy control P923 G62 Automatic corner
override P923
G63 Tapping mode P921 P922 P923 G64 Cutting mode G65 User macro
Simple call — Update modal only
(Coordinate rotation by program)
G66 User macro Modal call A
Update modal only (Coordinate rotation by program)
G66.1 User macro Modal call B
Update modal only (Coordinate rotation by program)
Update modal only (Coordinate rotation by program)
G67 User macro Modal call cancel
Update modal only after macro (Coordinate rotation by program)
Coordinate rotation by program ON
P921 P922 — G68
3-dimensional coordinate conversion ON
—
Coordinate rotation by program cancel
(3-dimensional coordinate conversion cancel)
— — G69
3-dimensional coordinate conversion cancel
— —
G73 Fixed cycle (Step) P922 P923 G74 Fixed cycle (Counter tap)
*incl: Synchronous tapping P922 P923
G76 Fixed cycle (Fine balling) P922 P923 G80 Fixed cycle cancel — P923 G81 Fixed cycle (Drill/spot
drill) P922 P923
G82 Fixed cycle (Drill/counter-balling)
P922 P923
G83 Fixed cycle (Deep hole drill)
P922 P923
G84 Fixed cycle (Tap) *incl: Synchronous tapping
P922 P923
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
469
Format Function
When this command is designated during
3-dimensional coordinate conversions
When 3-dimensional coordinate conversion is designated in this modal
status
When 3-dimensional coordinate conversion
is designated in the same block
G85 Fixed cycle (Balling) P922 P923 G86 Fixed cycle (Balling) P922 P923 G87 Fixed cycle (Back
balling) P922 P923
G88 Fixed cycle (Balling) P922 P923 G89 Fixed cycle (Balling) P922 P923 G90 Absolute value
command
G91 Incremental value command
G92 Coordinate system setting
P921 — P923
G94 Asynchronous feed (Feed per minute)
G95 Synchronous feed (Feed per revolution)
G96 Constant surface speed control ON
P921 P922 P923
G97 Constant surface speed control OFF
P921 — P923
G98 Fixed cycle (initial level return)
G99 Fixed cycle (R point level return)
(Note) All the G codes not listed above are disabled.
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
470
Relation with other functions
(1) Circular interpolation Circular interpolation in the 3-dimensional coordinate conversion modal functions according to the coordinate value resulted by the 3-dimensional coordinate conversion. With G17, G18 and G19 commands, circular interpolation functions normally for all the planes in which 3-dimensional coordinate conversion has been executed.
(2) Fine spline Specify a spline axis for the movement axis after the 3-dimensional coordinate conversion. When a movement occurs to the axis in which spline cannot be specified, spline will be in the pause status.
(3) Reference position check The 3-dimensional coordinate conversion is applied for the position for reference positioning specified with G27 command in the 3-dimensional coordinate conversion modal.
(4) Reference position return The 3-dimensional coordinate conversion is applied for the mid-point specified with G28, G30 command in the 3-dimensional coordinate conversion modal. However, reference position will be returned without the 3-dimensional coordinate conversion carried out.
(5) Tool position return 3-dimensional coordinate conversion is not carried out for the tool change position even if a command from G30.1 to G30.6 is issued in the 3-dimensional coordinate conversion modal. The return order and position will be the same as machine coordinate system.
(6) Tool compensation When executing the tool length/radius/position compensation in the 3-dimensional coordinate conversion modal, the 3-dimensional coordinate conversion is carried out after the compensation amount has been applied.
(7) Machine coordinate system selection Coordinate conversion will not be carried out for the machine coordinate system even if G53 command is issued in the 3-dimensional coordinate conversion modal.
(8) Mirror image When issuing the mirror image command in the 3-dimensional coordinate conversion modal, as well as when executing the 3-dimensional coordinate conversion in the mirror image modal, 3-dimensional coordinate conversion will be executed for the coordinate value, which is calculated by the mirror image.
(9) User macro When a user macro call command is issued in the 3-dimensional coordinate conversion modal, the 3-dimensional coordinate conversion will be valid after the macro execution.
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
471
(10) Fixed cycle for drilling The fixed cycle in the 3-dimensional coordinate conversion can be executed in an oblique direction for the orthogonal coordinate system. In the same manner, synchronous tapping cycle can also be executed. However, the mode for the fixed cycle for hole drilling will be changed from the rapid traverse to the cutting feed at the speed set with the parameter #1564 3Dspd. (Excluding during the synchronous tapping cycle.)
Move- ment 1
Move- ment 4
Move- ment 5
Move- ment 2
Initial position
R position
Movement 1: Position to the initial position at the rapid traverse. Movement 2: Position to the R point at the rapid at the rapid traverse. Movement 3: Hold drilling machining with the cutting feed. Movement 4: Recess to the R point
(Cutting feed or rapid traverse depending on the fixed cycle mode.)
Movement 5: Return to the initial position at the rapid traverse. Movement 2 to 5: Cutting feed set with the parameter #1564 3Dspd during
the 3-dimensional coordinate conversion. Move- ment 3
(11) Synchronous tapping cycle The Synchronous tapping cycle in the 3-dimensional coordinate conversion modal will not function even if #1223 BIT3 (synchronous tapping in-position check expansion valid) is valid. Set the synchronous tapping cycle to invalid.
(12) Geometric command Geometric command can be issued in the 3-dimensional coordinate conversion modal. However, if the geometric command is issued in the same block as in the 3-dimensional coordinate conversion command (G68.1, G69.1), P32 Illegal address will occur.
(13) Initial constant surface speed When the 3-dimensional coordinate conversion command is issued while the parameter initial constant surface speed is valid, P922 3D conversion illegal mode will occur. This is the same consequence as in the case where the 3-dimensional coordinate conversion command is issued in the constant surface speed (G96) modal.
(14) Machine lock The machine lock in the 3-dimensional coordinate conversion modal will be valid for the movement axis for the coordinate value after executing the 3-dimensional coordinate conversion.
(15) Interlock The interlock in the 3-dimensional coordinate conversion modal will be valid for the movement axis for the coordinate value after executing the 3-dimensional coordinate conversion.
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion ; G68/G69
472
(16) Coordinate read variable When reading the workpiece coordinate system/skip coordinate system during the 3-dimensional coordinate system conversion modal, local coordinate system and G68 program coordinate system can be switched with the parameter «#1563 3Dcdrc».
(17) Manual operation Manual operation in the 3-dimensional coordinate conversion modal will not execute the 3-dimensional conversion. Manual operation will be executed in the machine coordinate system. Also, when the manual ABS is OFF, G68 program coordinate system will move as much as the manual interruption or manual feed amount.
(18) Workpiece coordinate display Whether the workpiece coordinate position in the 3-dimensional coordinate conversion modal to be displayed in the workpiece coordinate system or in the G68 program coordinate system can be switched with the parameter #1561 3Dcdc. In the same manner, absolute value can be displayed on the special display.
(Note) 1um of display deviation may occur during the 3-dimensional coordinate conversion; however, this is normal.
(19) Remaining command display Whether the remaining commands in the 3-dimensional coordinate conversion modal to be displayed in the workpiece coordinate system or in the G68 program coordinate system can be switched with the parameter #1562 3Dremc.
(Note) 1um of display deviation may occur during the 3-dimensional coordinate conversion; however, this is normal.
(20) Others G41, G42, and the fixed cycle command G73 to G89 have to be nested inside the G68/G69 commands. For the block next to G68, a movement command in the G90 (Absolute value command) mode has to be issued. (Example)
G68 X50. Y100. Z150. I1 J0 K0 R60. ; G90 G00 X0 Y0 Z0 ; Issuance of G90 mode movement commands G41 D01 ;
G40 ; G69 ;
G00 command during 3-dimensional coordinate conversion modal is the interpolation type regardless of settings of the basic parameter #1086 G0Intp (G00 non-interpolation)
Origin zero cannot be executed during the 3-dimensional coordinate conversion modal.
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
473
13.24 Tool Center Point Control; G43.4/G43.5
Function and purpose
The tool center point control function controls a commanded position described in the machining program to be the tool center point in the coordinate system that rotates together with a workpiece (table coordinate system). This function can be applied for 5-axis machining, including a tool tilt type (Fig. 1 (a)) with two rotary axes set on the head, table tilt type (Fig. 1 (b)) with two rotary axes set on the table, or combined type (Fig. 1 (c)) with a rotary axis set on each tool and table. With this function, in the case of using tool tilt type, the tool center point is controlled so that it moves on the programmed path specified on the workpiece coordinate system. In the case of using the table tilt type, the tool center point is controlled so that it moves on the programmed path specified on the table coordinate system (a coordinate system which rotates together with a workpiece).
Tool center point control OFF and
tool length compensation along the tool axis ON Tool center point control ON
Rotation center Rotation center
Path of the tool center point
Controls so that the path of the tool holder center point draws a straight line.
Controls so that the path of the tool center point draws a straight line.
Fig.1(a)
Traces of the tool center point
Z(+)
X(+)
B(-)
Rotation center
Controls so that the tool holder center point positions on the workpiece coordinate system.
Controls so that the tool center point positions on the table coordinate system.
Fig.1(b)
B(-)
Z(+)
X(+)
X'(+) Z»(+)
X»(+)
Tool center point control OFF and tool length compensation along the tool axis ON
Tool center point control ON
Rotation center
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
474
Tool center point control OFF and tool length compensation along the tool axis ON
Tool center point control ON
Traces of the tool center point
Z(+)
X(+)
B(-)
Rotation center
Controls so that the tool holder center point positions on the workpiece coordinate system.
Controls so that the tool center point positions on the table coordinate system.
Fig.1(c)
B(-)
Z(+)
X(+)
X'(+) Z»(+)
X»(+)
Z'(+) Rotation center
To use this function, its dedicated option is required. Without the option, a program error (P940) occurs upon executing the tool center point control command.
Command format
There are two command formats: , where tool angle is commanded by the rotary axis; and , where tool angle is commanded by the vectors of the workpiece surface, I, J, and K.
(1) Tool Center Point Control ON
G43.4 (X__ Y__ Z__ A__ C__) H__; G43.5 (X__ Y__ Z__) I__ J__ K__ H__;
Tool center point control type1 ON Tool center point control type2 ON
G43.4 G43.5 X,Y,Z A,C I,J,K H
: Tool center point control type1 command : Tool center point control type2 command : Orthogonal coordinate axis movement command : Rotary axis movement command : Workpiece surface angle vector : Tool length offset number
(Note 1) When orthogonal coordinate axis movement command or rotary axis movement command is not issued in the same block, start-up without movement command is applied. (No movement for the offset amount.)
(Note 2) Commands to I, J, and K will be ignored during the tool center point control type1.
(Note 3) Rotary axis movement command cannot be executed during the tool center point control type2. If the command is issued, a program error (P33) occurs.
(Note 4) If I, J, or K is omitted when issuing the tool center point control type2 command, the omitted address will be considered as 0.
(2) Tool Center Point Control cancel
G49 (X__ Y__ Z__ A__ C__) ; Tool Center Point Control cancel (Note 1) Instead of using G49, the following G codes in the G group 8 can be used for canceling.
G43 (tool length compensation in the forward direction) / G44(Tool length offset in the reverse direction) / G43.1 (tool length compensation along the tool axis)
(Note 2) If orthogonal coordinate axis command and rotary axis command are issued in the same block as G49, the tool center point control modal will be canceled on the spot. Then, commanded axis movement will be performed. If G49 is issued alone, the tool center point control modal will be cancelled on the spot, and yet no axis movement (movement for the compensation amount) will be performed.
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
475
Programming coordinate system
The end position of each block looking from the programming coordinate system is specified in the tool center point control mode. In the program, specify the position of the tool center point. The programming coordinate system is a coordinate system used for the tool center point control, and is specified either the table coordinate system (a coordinate which rotates together with a workpiece) or the workpiece coordinate system by the parameter.
(1) Table coordinate system When 0 is specified for the programming coordinate system selection parameter, the table coordinate system, which is the valid workpiece coordinate system at that time fixed to the table, is specified as the programming coordinate system. Table coordinate system rotates along the table rotation and not the tool axis rotation. The subsequent X,Y,Z addresses are considered to have been issued on the table coordinate system. When a rotary axis movement is commanded in a block prior to G43.4/G43.5 command, the angle generated by rotary axis movement is regarded as an initial setting at G43.4/G43.5 command.
(2) Workpiece coordinate system
When 1 is specified for the programming coordinate system selection parameter, the programming coordinate system will be the valid workpiece coordinate system at that time. The coordinate system in this case does not rotate along the table rotation. A linear movement is carried out for the table (workpiece) when the subsequent X,Y,Z addresses are issued. The end position looking from the workpiece coordinate system after table rotation is specified to the X, Y and Z.
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
476
Start-up
(1) Start-up without movement command
(a) Tool center point control type1, type2 When the tool center point control is ON, no axis movement is performed (including movement for the compensation amount).
:
G43.4 Hh ; : or :
G43.5 Hh ;
Y
Z
A axis(+)
: G43.4 Hh ; : or : G43.5 Hh ; Y Z A axis(+) (b) Tool center point control type2 G43.5 Ii Jj Kk Hh ; performs the same movement as the tool center point control type1 in (2). (2) Start-up with movement command (When orthogonal coordinate axis command is issued in the same block) (a) Tool center point control type1, type2 When the tool center point control is ON, the tool center point moves only as much as it is ordered under the incremental value command. : G91 ; (Incremental value) G43.4 Yy Zz Hh; : or : G43.5 Yy Zz Hh ; : Y Z A axis(+) Y Z
: G91 ; (Incremental value) G43.4 Yy Zz Hh; : or : G43.5 Yy Zz Hh ; : Y Z A axis(+) Y Z Under the absolute value command, the tool center point moves to y1, z1. : G90 ; (Absolute value) G00 Yy0 Zz0; G43.4 Yy Zz Hh; : or : G43.5 Yy Zz Hh ; : Y Z A axis (+) y1-y0
: G90 ; (Absolute value) G00 Yy0 Zz0; G43.4 Yy Zz Hh; : or : G43.5 Yy Zz Hh ; : Y Z A axis (+) (y1,z1) h (y1,z1) h (y0,z0) y1-y0 z1-z0 z1-z0 (y0,z0) 13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 477 (b) Tool center point control type2 The rotary axis moves toward the commanded workpiece surface vector (I,J,K) direction along the movement command issued. z y (i,j,k) z y : G91 ; (Incremental value) G43.5 Yy Zz Ii Jj Kk Hh; : Y Z A axis (+)
: G91 ; (Incremental value) G43.5 Yy Zz Ii Jj Kk Hh; : Y Z A axis (+) (i,j,k) (3) Start-up with movement command (When rotary axis command is issued in the same block) (a) Tool center point control type1 In the case of using the tool tilt type, the orthogonal axis moves according to the rotary axis angle while fixing the tool center point to the center. In the case of using the table tilt type, the orthogonal axis moves so that the tool center point locates on the rotated table workpiece coordinate system. z a a : G43.4 Aa Hh; : Y Z A axis (+)
: G43.4 Aa Hh; : Y Z A axis (+) (b) Tool center point control type2 The program error (P33) will occur. 13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 478 Cancel (1) Cancellation without movement command (a) Tool center point control type1, type2 Cancellation movement for the compensation amount is not performed regardless of absolute/incremental value command. On the other hand, the tool center point control modal will be cancelled. No movement : G49; : Y Z A axis (+)
: G49; : Y Z A axis(+) No movement (2) Cancellation with movement command (When orthogonal coordinate axis command is issued in the same block) (a) Tool center point control type1, type2 Cancellation movement for the compensation amount is not performed regardless of absolute/incremental value command. Orthogonal coordinate axis movement command is executed upon cancellation of the tool center point control modal. z z y y : G91; (Incremental value) G49 Yy Zz ; : Y Z A axis (+)
: G91; (Incremental value) G49 Yy Zz ; : Y Z A axis (+) 13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 479 (3) Cancellation with movement command (When rotary axis command is issued in the same block) (a) Tool center point control type1, type2 Cancellation movement for the compensation amount is not performed regardless of absolute/incremental value command. Rotary axis movement command is executed upon cancellation of the tool center point control modal a a : G49 Aa Hh; : Y Z A axis (+)
: G49 Aa Hh; : Y Z A axis (+) During tool center point control (1) Tool center point control type1 (a) When executing movement command to the orthogonal coordinate axis and rotary axis. : G90 ; G43.4 Yy1 Zz1 Aa1 Hh ; Yy2 Aa2 ; Yy3 Aa3 ; : Tool center point moves on the tracks as programmed. Table coordinate system Z A axis(+) a1 z1 y1 y2 y3 a2=0 a3 Y (b) When executing movement command to the rotary axis only. : G90 ; G43.4 Yy1 Zz1 Aa1 Hh ; Yy2 ; Aa2 ; Yy3 Aa3 ; : When executing movement command to the rotary axis only, the orthogonal axis moves without moving the tool center point. Table coordinate system z1 a1 A axis (+) a2 a3 y1 y3y2 Z Y 13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 480 (2) Tool center point control type2 (a) When executing movement command to the orthogonal coordinate axis and workpiece surface angle vector command. Tool center point moves on the path as programmed. : G43.5 Yy1 Zz1 Ii1 Jj1 Kk1 Hh ; Yy2 Ii2 Jj2 Kk2 ; Yy3 Ii3 Jj3 Kk3 ; : Table coordinate system Z A axis (+) z1 y1 y2 y3 (i1,j1,k1) Y (i2,j2,k2) (i3,j3,k3) (b) When executing workpiece surface angle vector command only. : G43.5 Yy1 Zz1 Ii1 Jj1 Kk1 Hh ; Yy2 ; Ii2 Jj2 Kk2 ; Yy3 Ii3 Jj3 Kk3 ; : When executing workpiece surface angle vector command only, the orthogonal axis moves without moving the tool center point. Table coordinate system z1 (i1, j1, k1) A axis (+) a3 y1 y3y2 (i2, j2, k2) (i3, j3, k3) Z Y Feedrate during tool center point control Feedrate during the tool center point control is controlled so that the tool center point moves according to the commanded speed. 13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 481 Interpolation mode There are two modes of interpolation: single axis rotation interpolation and joint interpolation. You can select one of them by parameter. (1) Single axis rotation interpolation When transforming from a start-point angle vector «r1» into an end-point angle vector «r2», interpolate so that the angular rate of the rotary around the vector k axis, which is vertical to r1-r2 plane, will be constant. (a) Features Tool angle vector always exists on the plane consisting of O, r1 and r2. The angular rates of each rotary axis will not be constant. Z(-) Z’ (-) Y(-) Y'(-) Unit vector vertical to r1-r2 plane O Start-point command vector «r1» End-point command vector «r2» (b) Operations (Example) Current position Aa C0 When commanding G90 Yy A-a. C45. ; or G90 Yy Ii Jj Kk ; Y(-) Z(-)
Y(+)
Z(+)
Z(+)
Z»(+) Z'(+)
Y»(+
Y(+)
Y'(+)
Y(+)
Z(+)
Y(+)
Z(+) Z(+)
Z(+)
Y (+)
(2) Joint interpolation
A movement from a start-point angle vector «r1» to an end-point angle vector «r2» is interpolated to keep the angular rates of each axis constant.
(a) Features The angular rates of each rotary axis
become constant. As this control aims to keep the angular
rates of each rotary axis constant, a tool angle vector may not exist on the plane consisting of O, r1 and r2.
Y(-)
Start-point command vector «r1».
C(+)
A(+)
Z(-)
O
End-point command vector «r2».
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
482
Passing singular point
When passing the singular point (singular position*), there are two kinds of movements to be followed from the singular point. When using an A-C axis tilt type machinery, there are two different movements (Fig. b, c) to be followed. In those movements, the rotation angles of the A axis are the same absolute value but different in signs (+/-). The rotation angles of the C axis corresponding the two movements are differed by 180 degrees one another. Determine which one of the two movements are to be selected with parameter. The figures below are the example of movements seen during tool center point control type 2. When the tool center-point-side rotary axis moves in the sign (+) direction from the starting position (Fig. a), (Fig. b) is representing «passing singular point type1». When the tool center-point-side rotary axis moves in the sign (-) direction from the starting position (Fig. a), (Fig. c) is representing «passing singular point type2».
Y(-)
Z(-)
C0
Fig. a
(a) Movement in sign(+)
Y(-)
Z(-)
C0
Fig. b
(b) Movement in sign(-)
Y(-)
Z(-) —
C0
Fig. c
*The position in which the tool center-point-side rotary axis or the table base-side rotary axis is 0.
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
483
(1) Passing singular point type1 Select the same direction as the start point of the tool base-side rotary axis or table workpiece-side rotary axis in the block where a singular point passing is carried out. When the rotation angle of the start point is 0, select the wider stroke limit. When the stroke limits are the same, select the one with a minus-coded rotation angle.
X(-) C axis rotates 180 Y(-)
Z(-)
Singular point
When passing the neighborhood of the singular point, C axis rotates 180 within the parameter «#7907 CHK_ANG» (Judging angle for the singular point neighborhood.).
Fig. (a)
C axis rotates 180
Z(+) Z'(+)
Y(+) Y'(-)
Singular point
When passing the neighborhood of the singular point, C axis rotates 180 within the parameter «#7907 CHK_ANG» (Judging angle for the singular point neighborhood.).
Z»(+)
Y»(-)
Fig. (b)
Z(+)
C axis rotates 180
Y(-) Y(+)
Singular point
When passing the neighborhood of the singular point, C axis rotates 180 within the parameter «#7907 CHK_ANG» (Judging angle for the singular point neighborhood.).
Z(+) Z(+)
Y(-) Fig. (c)
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
484
(2) Passing singular point type 2
Select the one with the smaller rotary movement amount of the tool base-side rotary axis or the table workpiece-side rotary axis on the singular point. When the tool base-side rotary axis and the table workpiece have the same rotary movement amount, select the one with the tool base-side rotary axis or the table workpiece-side rotary axis that are to be rotated in the minus-coded direction.
X(-)
Y(-)
Z(-) Fig. (a)
C axis does not rotate 180 when passing the neighborhood of the singular point.
Z(+)
Z'(+)
Y(+) Y'(+) Y»(+)
Z»(+)
Fig. (b)
C axis does not rotate 180 when passing the neighborhood of the singular point.
Z(+)
Y(+) Y(+)
Z(+)
Y(+)
Z(+)
Fig. (c)
C axis does not rotate 180 when passing the neighborhood of the singular point.
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
485
(3) Movement in the singular point neighborhood in each interpolation mode
Inter- polation mode
Command Type of passing
sigular point
Command from a singular point to a non-singular point
Command to pass a singular point
Type 1 G43.4 (Rotary axis command) Type 2
Value as commanded. However, in the case where the signs at the start point and end point of either tool center-point-side rotary axis or table base-side rotary axis differ, if tool base-side rotary axis or table workpiece-side rotary axis rotates in the same block, the tool will not pass the singular point, resulting in a program error (P943).
Type 1 Select the one with the wider stroke range. When the stroke range is the same, select a minus direction of the tool center-point-side rotary axis or the table base-side rotary axis.
Select the one with the same-coded end point as the start point of the tool center-point-side rotary axis or the table base-side rotary axis.
Single axis rotation inter- polation
G43.5 (IJK command)
Type 2 Select the one with the smaller movement amount of the tool base side rotary axis or the table workpiece side rotary axis.
Type 1 G43.4 (Rotary axis command)
Type 2 Value as commanded.
Type 1 Select the one with the wider stroke range. When the stroke range is the same, select a minus direction of the tool center-point-side rotary axis or the table base-side rotary axis.
Select the one with the same-coded end point as the start point of the tool center-point-side rotary axis or the table base-side rotary axis.
Joint inter- polation
G43.5 (IJK command)
Type 2 Select the one with the smaller movement amount of the tool base-side rotary axis or the table workpiece-side rotary axis.
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
486
Rotary Axis Prefiltering
Rotary axis prefiltering means smoothing (prefiltering) the rotary axis command (tool angle shift) process, which moves the rotary axis smoothly and produces smoother cutting surface. Tool center point moves on the tracks as programmed by the rotary axis command while the command process is smoothed with this function. This function is available for the programs which have intermittent rotary axis commands (tool angle shifts) or the programs with inconstant shift amount of rotary axis angle (or tool angle) per unit time. Set the filter time constant for this function with parameters. When the rotary axis prefiltering is disabled, the tool center point shift speed may be sharply fluctuated due to the intermitted rotary axis command. See the following image.
Machine position(rotation center)
Without tool angle shift With tool angle shift
Tool center point Tool center point needs to be shifted at constant speed in spite of the tool angle shift.
P0 P1 P2 P3 P4 P5 P6 P7 P8 P9 P10 P11
Q1 Q2 Q3 Q4 Q5 Q6 Q7 Q8
Q9 Q10
As shown below, the rotary axis prefiltering reduces speed fluctuation of tool canter point by smoothing the rotary axis command process.
Machine position(rotation center)
Without tool angle shift
With tool angle shift
Tool center pointTool center point needs to be shifted at constant speed
P0 P1 P2 P3 P4 P5 P6 P7 P8 P9 P10 P11
Q1 Q2 Q3 Q4 Q5 Q6 Q7 Q8
Q9 Q10
Tool angle before smoothing
Tool angle after smoothing
This function is available only when SSS control is enabled. This function is disabled at G00 command. The actual angle of the tool may be deviated from the commanded one in the program.
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
487
Relation with other functions (Relation with other G codes)
Pxxx in the list indicates the program error Nos.
Format Function The function indicated at the left is commanded in the modal of this function
This function is commanded in the modal
indicated at the left
This function is commanded in the same
block G00 Positioning Switched to a rapid
traverse feed rate, and then tool center point Control is performed at the rate.
Perform tool center point control at a rapid traverse feed rate.
Perform tool center point control at a rapid traverse feed rate.
G01 Linear interpolation Switched to a cutting feed rate, and then tool center point control is performed at the rate.
Perform tool center point control at a cutting feedrate.
Perform tool center point control at a cutting feedrate.
Circular interpolation P942 P941 P941 G02/G03 G02/G03 Helical Interpolation P942 P941 P941
Spiral Interpolation P942 P941 P941 G02.1/G03.1 G02.3/G03.3 Exponential interpolation P942 P941 P941 G04 Dwell Dwelling is performed. — Tool center point control is
ignored as dwell function takes precedence over the tool center point control function.
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
488
Format Function The function indicated at the left is commanded in the modal of this function
This function is commanded in the modal
indicated at the left
This function is commanded in the same
block P1 (Note 1)
Max. feedrate is 16.8m/min when 1mm segment G1 block is commanded with 5 axes simultaneously
Max. feedrate is 16.8m/min when 1mm segment G1 block is commanded with 5 axes simultaneously
P33
P2 (Note 1)
High-speed machining mode
Max. feedrate is 100m/min when 1mm segment G1 block is commanded with 5 axes simultaneously
Max. feedrate is 100m/min when 1mm segment G1 block is commanded with 5 axes simultaneously
P33
G05
P10000 (Note 2)
High-speed high-accuracy control II
Max. feedrate is 100m/min when 1mm segment G1 block is commanded with 5 axes simultaneously
P941 P33
G05.1 (Note 2)
High-speed high-accuracy control I
Max. feedrate is 16.8m/min when 1mm segment G1 block is commanded with 5 axes simultaneously
Max. feedrate is 16.8m/min when 1mm segment G1 block is commanded with 5 axes simultaneously
P33
G06.2 NURBS interpolation P942 P*** NURBS general error P941 G07 Hypothetical axis
interpolation (Not implemented)
P942 — P941
G07.1 G107
Cylindrical Interpolation P942 P941 P941
P0 Tool center point control is performed in the cutting mode.
Tool center point control is performed in the cutting mode.
P33 G08 (Note 2)
P1
High-accuracy control
Tool center point control is performed in the high-accuracy control mode.
Tool center point control is performed in the high-accuracy control mode.
P33
G09 Exact Stop Check Deceleration check is performed at the block end.
— Deceleration check is performed at the block end.
G10/G11 Parameter input by program
P942 — P941
G10 Compensation data input by program
P942 — P941
G12/G13 Circular cutting P942 — Tool center point control is ignored as the circular cutting takes precedence over the tool center point control function.
G12.1/G13.1 G112/G113
Polar coordinate interpolation
P942 P941 P941
G15/G16 Polar coordinate command
P942 P941 P941
(Note 1) It is valid when the parameter «#1267 ext03/bit0» is OFF. If it is commanded when the
parameter is ON, the program error (P34) will occur. (Note 2) It is valid when the parameter «#1267 ext03/bit0» is ON. If it is commanded when the
parameter is OFF, the program error (P34) will occur.
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
489
Format Function The function indicated at the left is commanded in the modal of this function
This function is commanded in the modal
indicated at the left
This function is commanded in the same
block G17~G19 Plane selection The modal is switched to
the specified plane. — The modal is switched to
the specified plane. G20/G21 Inch / Metric P942 Tool center point control is
performed according to the inch / metric modal.
P941
G22/G23 Stroke check before travel
P942 P941 P941
G27 Reference position check
P942 — The tool center point control is ignored as the reference position check becomes valid.
G28 Reference position return
P942 — The tool center point control is ignored as the reference position return becomes valid.
G29 Start position return P942 — The tool center point control is ignored as the start position return becomes valid.
G30 2nd, 3rd, 4th reference position return
P942 — The tool center point control is ignored as the 2nd, 3rd, 4th reference position return becomes valid.
G30.1~G30.6 Tool change position return 1 to 6
P942 — P941
G31 Skip P942 — P941
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
490
Format Function The function indicated at the left is commanded in the modal of this function
This function is commanded in the modal
indicated at the left
This function is commanded in the same
block G31.1~G31.3 Multi-step skip function P942 — P941 G33 Thread cutting P942 P941 P941 G34~ G36/G37.1
Special Fixed Cycle P942 — P941
G37 Automatic tool length measurement
P942 — P941
G38 Tool radius compensation vector specification
P942 — P941
G39 Tool radius compensation corner circular command
P942 — P941
G40/G41/G42 Tool radius compensation
P942 P941 P941
G40.1/G41.1/G 41.2
Normal line control P942 P941 P941
G43/G44/G49 Tool length compensation
Tool length compensation can be performed upon tool center point control cancellation.
Tool center point control can be performed upon tool length compensation cancellation.
The subsequently commanded modal takes precedence.
G43.1/G49
Tool length compensation along the tool axis
Tool length compensation along the tool axis can be performed upon tool center point control cancellation.
Tool center point control can be performed upon tool length compensation along the tool axis cancellation.
The subsequently commanded modal takes precedence.
G45/G46/ G47/G48
Tool position offset P942 — P941
G50/G51 Scaling P942 P941 P942 G50.1/G51.1 Mirror image P942 P941 P941 G52 Local coordinate system
setting P942 — The tool center point
control is ignored as the local coordinate system setting becomes valid.
G53 Machine coordinate system selection
P942 — The tool center point control is ignored as the machine coordinate system selection becomes valid.
G54~G59/ G54.1
Workpiece coordinate system selection
P942 Tool center point control is performed in the currently selected workpiece coordinate system.
P941
G60 Unidirectional positioning
P942 — The tool center point control is ignored as the unidirectional positioning becomes valid.
G61 Exact stop check mode Deceleration check is performed at the block end.
Deceleration check is performed at the block end.
Deceleration check is performed at the block end.
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
491
Format Function The function indicated at the left is commanded in the modal of this function
This function is commanded in the modal
indicated at the left
This function is commanded in the same
block G61.1 High-accuracy control Tool center point control is
performed in the high-accuracy control mode.
Tool center point control is performed in the high-accuracy control mode.
Tool center point control is performed in the high-accuracy control mode.
G61.2 High-accuracy spline interpolation 1
P942 P941 P941
G62 Automatic corner override
P942 P941 P941
G63 Tapping mode P942 P941 P941 G64 Cutting mode Tool center point control is
performed in the cutting mode.
Tool center point control is performed in the cutting mode.
Tool center point control is performed in the cutting mode.
G65~ G67/G66.1
User macro Tool center point control becomes valid even in the user macro program.
Tool center point control becomes valid even in the user macro program.
Tool center point control is ignored as the user macro takes precedence over the tool center point control function.
— User macro subprogram termination
User macro subprogram is terminated.
— Tool center point control is ignored.
— End position error check cancellation
The end position error check cancellation becomes valid.
— Both end position error check cancellation and tool center position control become valid.
G68/G69 Coordinate rotation P942 P941 P941 G68IiJjKk/ G69
3-dimensional coordinate conversion
P922 P941 P923
G70~G89 Fixed cycle P942 The tool center point control is ignored as the start fixed cycle becomes valid.
The tool center point control is ignored as the start fixed cycle becomes valid.
G90/G91 Absolute/Incremental value command
The modal is switched to the specified absolute / incremental value command, and then tool center point control is performed.
Tool center point control is performed under the specified absolute / incremental value command.
Tool center point control is performed under the specified absolute / incremental value command.
G92 Machine coordinate system setting
P942 — P941
G94 Feed per minute Tool center point control is performed in the feed-per-minute mode.
Tool center point control is performed in the feed-per-minute mode.
Tool center point control is performed in the feed-per-minute mode.
G95 Feed per revolution P942 P941 P941 G96/G97 Constant surface speed
control P942 P941 P941
G98 Fixed cycle initial level return
The modal is switched to G98 and tool center point control becomes valid.
The modal is switched to G98 and tool center point control becomes valid.
The modal is switched to G98 and tool center point control becomes valid.
G99 Fixed cycle R point level return
The modal is switched to G99 and tool center point control becomes valid.
The modal is switched to G99 and tool center point control becomes valid.
The modal is switched to G99 and tool center point control becomes valid.
G114.1 Spindle synchronization P942 P941 P941 (Note) All the G codes not listed above are disabled.
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
492
Relation with other functions
(1) F 1-digit feed
Controls so that the tool center point moves at the commanded speed. Note that speed cannot be changed with the manual handle.
(2) Buffer correction
Buffer correction cannot be performed during tool center point control. (3) Miscellaneous functions (MSTB)
Miscellaneous function (MSTB) command can be executed during tool center point control. (When passing the singular point, strobe signal is output at the block start and the completion wait at the block end.)
(Example)
:
G90 Aa1 ;
G43.4 Yy1 Aa2 Mm Hh ;
:
M strobe output
Table workpiece coordinate system Y
Z A axis (+)
a
y1
M completion wait Passing sigular point
C axis (+)
a2
(4) Spindle/C axis control
Axes unrelated to the tool tilt or table tilt can be controlled. (5) Manual reference position return
Do not perform manual reference position return during tool center point control. If performed, the tool moves off the programmed track.
(6) Machining time calculation
Machining time calculation is not performed accurately on the machining program in which the cool center point control mode is commanded.
(7) Graphic trace
Graphic trace during the tool center point control allows the tool center point to be traced. (8) Graphic check
Graphic check during the tool center point control always allows the tool center point to be viewed for the purpose of programming confirmation.
(9) Program restart
Restart search cannot be performed during the tool center point control. If attempted, a program error (P49) occurs.
(10) Rest modal retention
Cancelled during the tool center point control.
(11) Collation stop Position in the tool center point control can be collated.
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
493
(12) Automatic operation handle interruption Do not perform the automatic operation handle interruption during the tool center point control. If performed, the tool moves off the programmed track.
(13) Manual / Automatic simultaneous
Manual / Automatic simultaneous cannot be executed to the axes related to the tool center point control during the tool center point control.
(14) Tool handle feed & interruption
Do not perform the tool handle feed & interruption during the tool center point control. If performed, the tool moves off the programmed track.
(15) Corner chamfering/Corner R
When the corner chamfering/corner R is performed during the tool center point control, the tool center point control becomes valid to the track after the corner chamfering/corner R.
(16) Mirror image by parameter setting / external mirror image input
When the tool center point control command is issued during the mirror image by parameter/external input, a program error (P941) occurs. Also, do not turn the mirror image by parameter/external input ON during the tool center point control.
(17) Linear angle command
When A axis is used as a rotary axis, the linear angle command cannot be executed. When A axis is not used as a rotary axis, tool center point control becomes valid to the shape after the linear angle command.
(18) Geometric command
When A axis is used as a rotary axis, the geometric command cannot be executed. If executed, a program error When A axis is not used as a rotary axis, tool center point control becomes valid to the shape after the geometric command.
(19) Figure rotation
The tool center point control becomes valid to the shape after the figure rotation.
(20) Coordinate rotation by parameter When the tool center point control command is issued during the coordinate rotation by parameter, a program error (P941) occurs. Also, do not turn the coordinate rotation by parameter ON during the tool center point control.
(21) Chopping
Chopping operation for the 3 orthogonal axes and 2 rotary axes cannot be performed during the tool center point control.
(22) Macro interruption
If the macro interruption command is executed during the tool center point control, a program error (P941) occurs.
(23) Tool life management
The compensation amount of the tool center point control during the tool life management is equal to the compensation amount of the tool subjected to the tool life management.
(24) G00 non-interpolation
Functions as G00 interpolation.
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5
494
(25) Actual feed rate display
The final combined feed rate is displayed here. (26) Manual interruption
When the manual interruption is executed during the feed hold or single block stop, the movement will be the one to be observed when the manual ABS is OFF when rebooting regardless of whether an absolute/incremental value command is selected.
(27) Machine lock
The each Machine Lock becomes valid to the motor axis. (28) Remaining distance counter
Remaining distance at the tool center point on the programming coordinate system is displayed.
(29) Interlock
Interlock is applied for the motor axis.
(30) Cutting feed / Rapid traverse override Override is applied to the feedrate at the tool center point. When the federate is clamped, the override is applied to the clamp speed.
(31) Manual reference position return
If the manual reference position return is performed during the tool center point control, the tool moves off the programmed track after that.
(32) Dry run
Dry run is applied to the speed at the tool center point.
(33) NC reset Immediately decelerates to stop when the NC reset is executed during the tool center point control. The tool center point control will be canceled even if NC reset 1 and the modal retention.
(34) Emergency stop
Immediately stops if the emergency stop is applied during the tool center point control.
(35) Stored stroke limit Stored stroke limit will be valid at the motor axis for all IB, IIB and IC.
(36) MDI interruption
When the MDI interruption is performed during the tool center point control, an operation error (O170) occurs.
13. Program Support Functions 13.25 Timing-synchronization between Part Systems
495
13.25 Timing-synchronization between Part Systems
CAUTION When programming a program of the multi-part system, carefully observe the movements caused by other part systems’ programs.
Function and purpose
The multi-axis, multi-part system complex control NC system can simultaneously run multiple machining programs independently. The timing-synchronization between part systems function is used in cases when, at some particular point during operation, the operations of 1st and 2nd part systems are to be synchronized or in cases when the operation of only one part system is required.
! ……;
! ……;
! ……;
%
! ……;
! ……;
! ……;
%
Simultaneous and independent operation
Timing-synchronization Simultaneous and independent operation
Timing-synchronization 2nd part system operation only; 1st part system synchronizing
Timing-synchronization Simultaneous and independent operation
2nd part system machining program1st part system machining program
No program
13. Program Support Functions 13.25 Timing-synchronization between Part Systems
496
Command format
!L__ ; L : Synchronizing No. 1 to 9999
$1 $2
!L1; !L1; Timing- synchro- nization
Detailed description
(1) If !L__ is commanded from one part system, operation of the first part system’s program will
wait until !L__ is commanded from the other part system’s program. When !L__ is commanded, the programs for the two part systems will start simultaneously.
1st part system
program 2nd part system program
Pi1 Pn1
Pn2Pi2
Pn1
Pi1 Pi2
Pn2
1st part system
2nd part system
Waiting
Starts simultaneously
Timing- synchronization
!L__;
!L__;
(2) The timing-synchronization command is normally issued in a single block. However, if a
movement command or M, S or T command is issued in the same block, whether to synchronize after the movement command or M, S or T command or to execute the movement command or M, S or T command after synchronization will depend on the parameter (#1093 Wmvfin).
#1093 Wmvfin 0: Synchronize before executing movement command. 1: Synchronize after executing movement command.
13. Program Support Functions 13.25 Timing-synchronization between Part Systems
497
(3) If there is no movement command in the same block as the timing-synchronization command, when the next block movement starts, timing-synchronization may not be secured between the part systems. To synchronize the part systems when movement starts after the timing-synchronization, issue the movement command in the same block as the synchronizing command.
(4) Timing-synchronizing is done only while the part system to be synchronized is operating automatically. If this is not possible, the timing-synchronization command will be ignored and operation will advance to the next block.
(5) The L command is the synchronizing identification No. The same Nos. are synchronized but when they are omitted, the Nos. are handled as L0.
(6) «SYN» will appear in the operation status section during timing-synchronization. The timing-synchronization signal will be output to the PLC I/F.
Example of timing-synchronization between part systems
$1 $2
P11
!L1;
P12
!L2;
P13
P21
!L1;
P22
P23
!L2;
P24
The above programs are executed as follows:
$2
$1 P11
P21
L1 L2
P12 P13
P24 P23P22
14. Coordinates System Setting Functions 14.1 Coordinate Words and Control Axes
498
14. Coordinates System Setting Functions 14.1 Coordinate Words and Control Axes
Function and purpose
There are three controlled axis for the basic specifications, but when an additional axis is added, up to four axes can be controlled. Pre-determined alphabetic coordinate words that correspond to the axes are used to designate each machining direction.
For XY table
Program coordinates
Table movement direction
Table movement direction
Bed
XY table
+Z
+Z +Y
+X
+X +Y
Workpiece
For XY table
Program coordinates Table movement direction Table rotation direction
+Z +C
+X +X
+Y
+Y
+C
Workpiece
For XY and rotary table
14. Coordinates System Setting Functions 14.2 Basic Machine, Workpiece and Local Coordinate Systems
499
14.2 Basic Machine, Workpiece and Local Coordinate Systems
Function and purpose
The basic machine coordinate system is fixed in the machine and it denotes that position which is determined inherently by the machine. The workpiece coordinate systems are used for programming and in these systems the reference position on the workpiece is set as the coordinate zero point. The local coordinate systems are created on the workpiece coordinate systems and they are designed to facilitate the programs for parts machining.
R#1
Reference position
M
W1 W2
Local coordinate system
W4 (Workpiece 4 coordinate system)
M
R#1
W3 (Workpiece 3 coordinate system)
W1 (Workpiece 1 coordinate system)
W2 (Workpiece 2 coordinate system)
(Basic machine coordinate system)
14. Coordinates System Setting Functions 14.3 Machine Zero Point and 2nd, 3rd, 4th Reference Positions
500
14.3 Machine Zero Point and 2nd, 3rd, 4th Reference Positions
Function and purpose
The machine zero point serves as the reference for the basic machine coordinate system. It is inherent to the machine and is determined by the reference (zero) position return. 2nd, 3rd and 4th reference positions relate to the position of the coordinates which have been set beforehand by parameter from the zero point of the basic machine coordinate system.
2nd reference position Basic machine coordinate system Machine zero point
Local coordinate system
Workpiece coordinate system
1st reference position 3rd reference position
4th reference position
(G54 to G59)
(X1,Y1)
G52
x
y
x
y
x
y (X2,Y2)
14. Coordinates System Setting Functions 14.4 Basic Machine Coordinate System Selection; G53
501
14.4 Basic Machine Coordinate System Selection; G53
Function and purpose
The basic machine coordinate system is the coordinate system that expresses the position (tool change position, stroke end position, etc.) that is characteristic to the machine. The tool is moved to the position commanded on the basic machine coordinate system with the G53 command and the coordinate command that follows.
Command format
Basic machine coordinate system selection
(G90) G53 X__ Y__ Z__ __ ; :Additional axis
Detailed description
(1) When the power is switched on, the basic machine coordinate system is automatically set as
referenced to the reference (zero) position return position, which is determined by the automatic or manual reference (zero) position return.
(2) The basic machine coordinate system is not changed by the G92 command. (3) The G53 command is valid only in the block in which it has been designated. (4) In the incremental value command mode (G91), the G53 command provides movement with
the incremental value in the coordinate system being selected. (5) Even if G53 is commanded, the tool radius compensation amount for the commanded axis will
not be canceled. (6) The 1st reference position coordinate value indicates the distance from the basic machine
coordinate system 0 point to the reference position (zero point) return position. (7) The G53 command will move with cutting feedrate or rapid traverse following command
modal. (8) If the G53 command and G28 command (reference position return) are issued in the same
block, the command issued last will be valid.
Basic machine coordinate system zero point
(500,500)
1st reference position coordinates X = +500 Y = +500
Reference (zero) position return position (#1)
-Y
-X R#1M
14. Coordinates System Setting Functions 14.5 Coordinate System Setting ;G92
502
14.5 Coordinate System Setting ;G92
Function and purpose
By commanding G92, the absolute value (workpiece) coordinate system and current position display value can be preset in the command value without moving the machine.
Command format
G92 X__ Y__ Z__ __ ; :Additional axis
Detailed description
[Position] X 0.000 Y 0.000 [Workpiece] X 300.000 Y 200.000
Reference position return completed
Power ON position
Power ON position
WG54 100. 200.
100.Reference position return
R,M R
Workpiece coordinate system
The basic machine coordinate system and workpiece coordinate system are created at the preset position.
[Position] X -200.000 Y -150.000 [Workpiece] X 100.000 Y 50.000
[Position] X 0.000 Y 0.000 [Workpiece] X 0.000 Y 0.000
Coordinate system setting
[Tool position]
WG54’100. 200.
WG54 100. 200. 300.
200. 100. 50.
100.
-100
-50. WG54
R,M R,M
For example, if G92X 0 Y 0; is commanded, the workpiece coordinate system will be newly created.
[Tool position]
Basic machine coordinate system
(2) By commanding G92, the absolute value (workpiece) coordinate system and current position display value can be preset in the command value without moving the machine.
(1) After the power is turned on, the first reference position return will be done with dog-type, and when completed, the coordinate system will be set automatically. (Automatic coordinate system setting)
(Note) If the workpiece coordinate system deviated because the axis is moved manually when
the manual absolute position switch is OFF, etc., the workpiece coordinate system can be corrected with the following steps. (1) Execute reference position return while the coordinate system is deviated. (2) After that, command G92G53X0Y0Z0;. With this command, the workpiece coordinate
position and current position will be displayed, and the workpiece coordinate system will be preset to the offset value.
14. Coordinates System Setting Functions 14.6 Automatic Coordinate System Setting
503
14.6 Automatic Coordinate System Setting
Function and purpose
This function creates each coordinate system according to the parameter values input beforehand from the setting and display unit when the reference position is reached with the first manual reference position return or dog-type reference position return when the NC power is turned ON.
Basic machine coordinate Machine zero point
1st reference position Workpiece
coordinate system 3 (G56)
Workpiece coordinate system 2 (G55)
Workpiece coordinate system 1 (G54)
Workpiece coordinate system 6 (G59)
Workpiece coordinate system 5 (G58)
Workpiece coordinate system 4 (G57)
y3 y2
y1
y4
x1
x3 x2
x4
Detailed description
(1) The coordinate systems created by this function are as follow:
(a) Basic machine coordinate system (b) Workpiece coordinate systems (G54 to G59)
(2) The parameters related to the coordinate system all provide the distance from the zero point of the basic machine coordinate system. Therefore, it is decided at which position in the basic machine coordinate system the first reference position should be set and then the zero point positions of the workpiece coordinate systems are set.
(3) When the automatic coordinate system setting function is executed, shifting of the workpiece coordinate system with G92, setting of the local coordinate system with G52, shifting of the workpiece coordinate system with origin set, and shifting of the workpiece coordinate system with manual interruption will be canceled.
(4) The dog-type reference position return will be executed in the following conditions. The first manual reference position return after power ON. The first automatic reference position return after power ON. The second and following manual reference position return when the dog-type is selected
with a parameter. The second and following automatic reference position return when the dog-type is selected
with a parameter.
14. Coordinates System Setting Functions 14.7 Reference (Zero) Position Return; G28, G29
504
14.7 Reference (Zero) Position Return; G28, G29
Function and purpose
(1) After the commanded axes have been positioned by G0, they are returned respectively at
rapid traverse to the first reference (zero) position when G28 is commanded. (2) By commanding G29, the axes are first positioned independently at high speed to the G28 or
G30 intermediate point and then positioned by G0 at the commanded position.
Reference position Machine zero point(0,0,0,0)
G28 G28
G29
G29
G30 G30P3
G30P4
G30P2
(x1,y1,z1,1) Intermediate point
(x2,y2,z2,2)
Start point
3rd reference position 4th reference position
(x3,y3,z3,3)
2nd reference position
Command format
G28 Xx1 Yy1 Zz1 1 ; Automatic reference position return G29 Xx2 Yy2 Zz2 2 ; Start position return 1/2 : additional axis
14. Coordinates System Setting Functions 14.7 Reference (Zero) Position Return; G28, G29
505
Detailed description
(1) The G28 command is equivalent to the following: G00 Xx1 Yy1 Zz1 1 ;
G00 Xx3 Yy3 Zz3 3 ; In this case, x3, y3, z3 and 3 are the reference position coordinates and they are set by a parameter «#2037 G53ofs» as the distance from the zero point of the basic machine coordinate system.
(2) After the power has been switched on, the axes which have not been subject to manual reference (zero) position are returned by the dog type of return just as with the manual type. In this case, the return direction is regarded as the command sign direction. If the return type is straight-type return, the return direction will not be checked. For the second and subsequence returns, the return is made at high speed to the reference (zero) position which was stored at the first time and the direction is not checked.
(3) When reference (zero) position return is completed, the zero point arrival output signal is output and also #1 appears at the axis name line on the setting and display unit screen.
(4) The G29 command is equivalent to the following: G00 Xx1 Yy1 Zz1 1 ;
G00 Xx2 Yy2 Zz2 2 ;
Rapid traverse (non-interpolation type) applies independently for each axis for the positioning from the reference position to the intermediate point.
In this case, x1, y1, z1 and 1 are the coordinates of the G28 or G30 intermediate point. (5) Program error (P430) results when G29 is executed if automatic reference (zero) position
return (G28) is not performed after the power has been switched on. (6) When the Z axis is canceled, the movement of the Z axis to the intermediate point will be
ignored, and only the position display for the following positioning will be executed. (The machine itself will not move.)
(7) The intermediate point coordinates (x1, y1, z1, 1) of the positioning point are assigned by the position command modal. (G90, G91).
(8) G29 is valid for either G28 or G30 but the commanded axes are positioned after a return has been made to the latest intermediate point.
(9) The tool compensation will be canceled during reference position return unless it is already canceled, and the compensation amount will be cleared.
14. Coordinates System Setting Functions 14.7 Reference (Zero) Position Return; G28, G29
506
Example of program
1st operation after power has been switched on
2nd and subsequent operations
2nd and subsequent operations
1st operation after power has been switched on
Rapid traverse rate
Near-point dog Reference (zero) position (#1)
(x1,z1) Intermediate point
Reference (zero) position (#1)
R
R
Return start position
G0Xx3Zz3;
G0Xx1 Zz1;
(Example1) G28 Xx1 Zz1 ;
14. Coordinates System Setting Functions 14.7 Reference (Zero) Position Return; G28, G29
507
Present position R
(Example2) G29 Xx2 Zz2 ;
(G0)Xx1 Zz1 ;
G28, G30 intermediate point (x1, z1)
G0 Xx2 Zz2 ;
(x2,z2)
Reference (zero) position (#1) Present position
Old intermediate point
(x1,z1)
C
G29 B
G28
A
D G30
New intermediate point
(x3,z3)
2nd reference (zero) position (#2)
R1
R2
(x2,z2)
(Example 3) G28 Xx1 Zz1 ; (From point A to reference (zero) position) G30 Xx2 Zz2 ; (From point B to 2nd reference (zero) position) G29 Xx3 Zz3 ; (From point C to point D)
14. Coordinates System Setting Functions 14.8 2nd, 3rd and 4th Reference (Zero) Position Return ; G30
508
14.8 2nd, 3rd and 4th Reference (Zero) Position Return; G30
Function and purpose
The tool can return to the second, third, or fourth reference (zero) position by specifying G30 P2 (P3 or P4).
2nd reference position Reference position
G28 G28
G29
G29
G30 G30P3
G30P4
G30P2
(x1,y1,z1,1) Intermediate point
Start point
3rd reference position 4th reference position
Command format
G30 P2 (P3, P4) Xx1 Yy1 Zz1 1;
1 : Additional axis
14. Coordinates System Setting Functions 14.8 2nd, 3rd and 4th Reference (Zero) Position Return ; G30
509
Detailed description
(1) The second, third, or fourth reference (zero) position return is specified by P2, P3, or P4. A
command without P or with P0, P1, P5 or a greater P number is ignored, returning the tool to the second reference (zero) position.
(2) In the second, third, or fourth reference (zero) position return mode, as in the first reference (zero) position return mode, the tool returns to the second, third, or fourth reference (zero) position via the intermediate point specified by G30.
(3) The second, third, and fourth reference (zero) positions coordinates refer to the positions specific to the machine, and these can be checked with the setting and display unit.
(4) If G29 is specified after completion of returning to the second, third, and fourth reference (zero) positions, the intermediate position used last is used as the intermediate position for returning by G29.
Intermediate point (x1,y1) 1st reference (zero) position
3rd reference (zero) position
R#3 (x2,y2)
G29Xx2Yy2;
R#1
G30P3Xx1Yy1;
-X
-Y
(5) With reference (zero) position return on a plane during compensation, the tool moves without
tool radius compensation from the intermediate point. With a subsequent G29 command, the tool moves with tool radius compensation until the G29 command from the intermediate point.
Tool nose center path
Programmed path
Intermediate point 3rd reference (zero) position
R#3
(x2,y2)
G29Xx2Yy2;
(x1,y1)
-Y
-X
G30P3Xx1Yy1;
14. Coordinates System Setting Functions 14.8 2nd, 3rd and 4th Reference (Zero) Position Return ; G30
510
(6) The tool length compensation amount for the axis involved is canceled after the second, third
and fourth reference (zero) position returns. (7) With second, third and fourth reference (zero) position returns in the machine lock status,
control from the intermediate point to the reference (zero) position will be ignored. When the designated axis reaches as far as the intermediate point, the next block will be executed.
(8) With second, third and fourth reference (zero) position returns in the mirror image mode, mirror image will be valid from the start point to the intermediate point and the tool will move in the opposite direction to that of the command. However, mirror image is ignored from the intermediate point to the reference (zero) position and the tool moves to the reference (zero) position.
X-axis mirror image
No mirror image
3rd reference (zero) position
R#3
-Y
-X
G30P3Xx1Yy1;
14. Coordinates System Setting Functions 14.9 Reference Position Check ; G27
511
14.9 Reference Position Check; G27
Function and purpose
This command first positions the tool at the position assigned by the program and then, if that positioning point is the first reference position, it outputs the reference position arrival signal to the machine in the same way as with the G28 command. Therefore, when a machining program is prepared so that the tool will depart from the first reference position and return to the first reference position, it is possible to check whether the tool has returned to the reference position after the program has been run.
Command format
G27 X__ Y__ Z__ P__ ; G27 X Y Z P
: Check command : Return control axis : Check number P1 : 1st reference position check P2 : 2nd reference position check P3 : 3rd reference position check P4 : 4th reference position check
Detailed description
(1) If the P command has been omitted, the first reference position will be checked. (2) The number of axes whose reference positions can be checked simultaneously depends on
the number of axes which can be controlled simultaneously. Note that the display shows one axis at a time from the final axis. (3) An alarm will occur if the reference position is not reached after the command is completed.
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset
512
14.10 Workpiece Coordinate System Setting and Offset ; G54 to G59 (G54.1)
Function and purpose
(1) The workpiece coordinate systems facilitate the programming on the workpiece, serving the reference position of the machining workpiece as the zero point.
(2) These commands enable the tool to move to the positions in the workpiece coordinate system. There are 6 workpiece coordinate systems which are used by the programmer for programming. (G54 to G59) In addition to the six sets of workpiece coordinate systems between G54 and G59, there are 48 or 96 additional workpiece coordinate system sets. (The 48 sets and 96 sets are optional specifications.)
(3) By these commands, the workpiece coordinate system will be re-set so that the present position of the tool on the current workpiece coordinate system become the commanded coordinates. (The «present position of the tool» includes the compensation amounts for tool radius, tool length and tool position.)
(4) An imaginary machine coordinate system with coordinates which have been commanded by the present position of the tool is set by this command.
(The «present position of the tool» includes the compensation amounts for tool diameter, tool length and tool position compensation.) (G54, G92)
Command format
(1) Workpiece coordinate system selection (G54 to G59)
(G90) G54 X__ Y__ Z__ __; : Additional axis
(2) Workpiece coordinate system setting (G54 to G59)
(G54) G92 X__ Y__ Z__ __; : Additional axis
(3) Extended workpiece coordinate system selection (P1 to P48 or P1 to P96) G54.1 Pn ;
(4) Extended workpiece coordinate system setting (P1 to P48 or P1 to P96) G54.1 Pn ; G92 X__ Y__ Z__ ;
(5) Extended workpiece coordinate system offset amount setting (P1 to P48 or P1 to P96) When the designated extended workpiece coordinate system offset amount is rewritten G10 L20 Pn X__ Y__ Z__ ;
When the extended workpiece coordinate system is selected, and the offset amount is rewritten G10 G54.1 Pn X__ Y__ Z__ ;
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset
513
Detailed description
(1) The tool radius compensation amounts for the commanded axes will not be canceled even if workpiece coordinate system is switched with any of the G54 through G59 or G54.1P1 through G54.1P96 commands
(2) The G54 workpiece coordinate system is selected when the power is switched ON.
(3) Commands G54 through G59 and G54.1P1 through G54.1P96 are modal commands (group 12).
(4) The coordinate system will move with G92 in a workpiece coordinate system.
(5) The offset setting in a workpiece coordinate system denotes the distance from the zero point of the basic machine coordinate system.
G55 reference position (zero point)
Reference position (zero point) return position
Basic machine coordinate system zero point
G54 reference position (zero point)
G54 X = 500 Y = 500 G55 X = 2000 Y = 1000
R#1
-X
-Y
-X(G54)(-500, -500)
-X(G55)(-2000, -1000)
W2 -Y(G55)
W1 -Y (G54)
M (#1)
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset
514
(6) The offset settings of workpiece coordinate systems can be changed any number of times. (They can also be changed by G10 L2(L20) Pp1 Xx1 Zz1.)
Handling when L or P is omitted G10 L2 Pn Xx Yy Zz ; n=0 : Set the offset amount in the external workpiece
coordinate system. n=1 to 6 : Set the offset amount in the designated workpiece
coordinate system. Others : The program error (P35) will occur.
G10 L2 Xx Yy Zz ; Set the offset amount in the currently selected workpiece coordinate system. When in G54.1 modal, the program error (P33) will occur.
G10 L20 Pn Xx Yy Zz ; n=1 to 96 : Set the offset amount in the designated workpiece coordinate system.
Others : The program error (P35) will occur. G10 L20 Xx Yy Zz ; Set the offset amount in the currently selected workpiece
coordinate system. When in G54 to G59 modal, the program error (P33) will occur.
G10 Pn Xx Yy Zz ; Set the offset amount in the designated coordinate system No. by P code. When the currently selected coordinate system is G54 to G59, P1 to P6 corresponds to G54 to G59 respectively. When the external coordinate system is selected, P No. corresponds to G54.1 P1 to P96. If other values are set, the program error (P35) will occur.
G10 Xx Yy Zz ; Set the offset amount in the currently selected coordinate system.
G10 G54.1 Xx Yy Zz ; When there is no P code in the same block as G54.1, the program error (P33) will occur.
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset
515
(7) A new workpiece coordinate system 1 is set by issuing the G92 command in the G54 (workpiece coordinate system 1) mode. At the same time, the other workpiece coordinate systems 2 through 6 (G55 to G59) will move in parallel and new workpiece coordinate systems 2 through 6 will be set.
(8) An imaginary machine coordinate system is formed at the position which deviates from the new workpiece reference (zero) position by an amount equivalent to the workpiece coordinate system offset amount.
Old workpiece 1 (G54) coordinate system
Old workpiece 2 (G55) coordinate system
New workpiece 1 (G54) coordinate system
New workpiece 2 (G55) coordinate system
Reference (zero) position return position
Basic machine coordinate system zero point
Imaginary machine coordinate system coordinate point based on G92
R#1 -X
-X(G54)
-X
-X(G54′)
-X(G55)
-X(G55′) -Y(G54)
-Y
-Y(G55)
-Y
-Y(G54′) -Y(G55′)
W2 W1
[W2]
[W1]
M
[M]
After the power has been switched on, the imaginary machine coordinate system is matched with the basic machine coordinate system by the first automatic (G28) or manual reference (zero) position return.
(9) By setting the imaginary basic machine coordinate system, the new workpiece coordinate system will be set at a position which deviates from that imaginary basic machine coordinate system by an amount equivalent to the workpiece coordinate system offset amount.
(10) When the first automatic (G28) or manual reference (zero) position return is completed after the power has been switched on, the basic machine coordinate system and workpiece coordinate systems are set automatically in accordance with the parameter setting.
(11) If G54X-Y-; is commanded after the reference position return (both automatic or manual) executed after the power is turned ON, the program error (P62) will occur. (A speed command is required as the movement will be controlled with the G01 speed.)
(12) Do not command a G code for which a P code is used in the same block as G54.1. The P code will be used in the prioritized G command.
(13) When number of workpiece offset sets additional specifications is not added, the program error (P39) will occur when the G54.1 command is executed. This error will also occur when one of P49 to P96 is commanded although the specifications allow up to the 48 sets.
(14) When number of workpiece offset sets additional specifications is not added, the program error (P172) will occur when the G10 L20 command is executed.
(15) The local coordinate system cannot be used during G54.1 modal. The program error (P438) will occur when the G52 command is executed during G54.1 modal.
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset
516
(16) A new workpiece coordinate system P1 can be set by commanding G92 in the G54.1 P1 mode. However, the workpiece coordinate system of the other workpiece coordinate systems G54 to G59, G54.1 and P2 to P48 will move in parallel with it, and a new workpiece coordinate system will be set.
(17) The offset amount of the extended workpiece coordinate system is assigned to the variable number as shown in Table 1.
(18) When the parameter #1151 Reset ini is OFF, the modal of G54.1 command will be retained even if the reset 1 is carried out.
(19) P address (coordinate system selection) of G54.1 cannot be commanded alone even in G54.1 modal. Even if commanded, the designated extended workpiece coordinate system cannot be selected. (Ex) P54.1 P5; Changed to P5 workpiece coordinate system. P3; Ignored. G92 X0 Y0 Z0; The current position becomes the zero point of P5 workpiece
coordinate system.
(20) When G92 is commanded in the extended workpiece coordinate system, the coordinate system will be sifted.
Table 1 Variable numbers of the extended workpiece coordinate offset system
1st axis to nth axis
1st axis to nth axis
1st axis to nth axis
1st axis to nth axis
P 1 #7001 to #700n P25 #7481 to #748n P49 #7961 to #796n P73 #7001 to #700n P 2 #7021 to #702n P26 #7501 to #750n P50 #7981 to #798n P74 #7021 to #702n P 3 #7041 to #704n P27 #7521 to #752n P51 #8001 to #800n P75 #7041 to #704n P 4 #7061 to #706n P28 #7541 to #754n P52 #8021 to #802n P76 #7061 to #706n P 5 #7081 to #708n P29 #7561 to #756n P53 #8041 to #804n P77 #7081 to #708n P 6 #7101 to #710n P30 #7581 to #758n P54 #8061 to #806n P78 #7101 to #710n P 7 #7121 to #712n P31 #7601 to #760n P55 #8081 to #808n P79 #7121 to #712n P 8 #7141 to #714n P32 #7621 to #762n P56 #8101 to #810n P80 #7141 to #714n P 9 #7161 to #716n P33 #7641 to #764n P57 #8121 to #812n P81 #7161 to #716n P10 #7181 to #718n P34 #7661 to #766n P58 #8141 to #814n P82 #7181 to #718n P11 #7201 to #720n P35 #7681 to #768n P59 #8161 to #816n P83 #7201 to #720n P12 #7221 to #722n P36 #7701 to #770n P60 #8181 to #818n P84 #7221 to #722n P13 #7241 to #724n P37 #7721 to #772n P61 #8201 to #820n P85 #7241 to #724n P14 #7261 to #726n P38 #7741 to #774n P62 #8221 to #822n P86 #7261 to #726n P15 #7281 to #728n P39 #7761 to #776n P63 #8241 to #824n P87 #7281 to #728n P16 #7301 to #730n P40 #7781 to #778n P64 #8261 to #826n P88 #7301 to #730n P17 #7321 to #732n P41 #7801 to #780n P65 #8281 to #828n P89 #7321 to #732n P18 #7341 to #734n P42 #7821 to #782n P66 #8301 to #830n P90 #7341 to #734n P19 #7361 to #736n P43 #7841 to #784n P67 #8321 to #832n P91 #7361 to #736n P20 #7381 to #738n P44 #7861 to #786n P68 #8341 to #834n P92 #7381 to #738n P21 #7401 to #740n P45 #7881 to #788n P69 #8361 to #836n P93 #7401 to #740n P22 #7421 to #742n P46 #7901 to #790n P70 #8381 to #838n P94 #7421 to #742n P23 #7441 to #744n P47 #7921 to #792n P71 #8401 to #840n P95 #7441 to #744n P24 #7461 to #746n P48 #7941 to #794n P72 #8421 to #842n P96 #7461 to #746n
CAUTION
If the workpiece coordinate system offset amount is changed during single block stop, the new setting will be valid from the next block.
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset
517
Example of program
(Example 1)
Present position
Reference (zero) position return position (#1)
R#1
(1)
M(2) (3)
(1) G28 X0Y0 ; (2) G53 X-1000 Y-500 ; (3) G53 X0Y0 ;
When the first reference position coordinate is zero, the basic machine coordinate system zero point and reference (zero) position return position (#1) will coincide.
(Example 2)
Present position
M -500
-1000
-1500
-X(G55)
-1000 -500
-Y (G54)
-Y (G55)
W2 -500
(11) (6)
(5) (4)
(3)
(2) (1)
(10) (7)
(8)(9)
(1) G28X0Y0 ; (2) G90G00G53X0Y0 ; (3) G54X-500 Y500 ; (4) G01G91X500F 100 ; (5) Y500 ; (6) X+500 ; (7) Y+500 ; (8) G90G00G55X0Y0 ; (9) G01X500 F200 ; (10) X0Y500 ; (11) G90G28X0Y0 ;
-X(G54)
Reference (zero) position return position (#1)
W1
-1000
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset
518
(Example 3) When workpiece coordinate system G54 has shifted (500, 500) in example 2 (It is
assumed that (3) through (10) in example 2 have been entered in subprogram 01111.) (1) G28 X0 Y0 ; (2) G90 G53 X0 Y0 ; (This is not required when there is no G53 offset.)
(3) G54 X -500Y-500 ; Amount by which workpiece coordinate system deviates
(4) G92 X0 Y0 ; New workpiece coordinate system is set. (5) M98 P1111 ;
New G55 coordinate system
(#1) Reference (zero) position return position
Present position
Old G55 coordinate system Old G54 coordinate system
M
-X(G55) -X
-Y (G54)
-Y (G55)
-X(G55′)
-Y (G54′)
-Y(G55′)
-Y
-X
-X(G54)
W2
W1 (4)
(3)
(2) (1)
(G54′) New G54 coordinate system
(Note) The workpiece coordinate system will shift each time steps (3) through (5) are repeated. The reference position return (G28) command should therefore be issued upon completion of the program.
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset
519
(Example 4) When six workpieces are placed on the same coordinate system of G54 to G59, and
each is to be machined with the same machining.
(1) Setting of workpiece offset data Workpiece1 X = -100.000 Y = -100.000 …………………………………. G54
2 X = -100.000 Y = -500.000 ………………………………… G55 3 X = -500.000 Y = -100.000 ………………………………… G56 4 X = -500.000 Y = -500.000 ………………………………… G57 5 X = -900.000 Y = -100.000 ………………………………… G58 6 X = -900.000 Y = -500.000 …………………………………. G59
(2) Machining program (subprogram)
O100; N1 G90 G0 G43X-50. Y-50. Z-100. H10; Positioning N2 G01 X-200. F50; Y-200. ;
X- 50. ; Y- 50. ;
N3 G28 X0 Y0 Z0 ;
~ N4 G98 G81 X-125. Y-75. Z-150. R-100. F40; 1 X-175. Y-125. ; 2 X-125. Y-175. ; 3 X- 75. Y-125. ; 4 G80; N5 G28 X0 Y0 Z0 ;
~ N6 G98 G84 X-125. Y-75. Z-150. R-100. F40 ; 1 X-175. Y-125. ; 2 X-125. Y-175. ; 3 X- 75. Y-125. ; 4
G80; M99;
Tapping
Surface cutting
Drilling
(3) Positioning program (main) G28 X0 Y0 Z0 ; When power is turned ON N1 G90 G54 M98 P100 ; N2 G55 M98 P100 ; N3 G57 M98 P100 ; N4 G56 M98 P100 ; N5 G58 M98 P100 ; N6 G59 M98 P100 ; N7 G28 X0 Y0 Z0 ; N8 M02 ; %
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset
520
W 2
-X
-Y
G 55
(W or
kp ie
ce 2
)
W 4
-X
-Y
G 57
(W or
kp ie
ce 4
)
W 6
-X
-Y
G 59
(W or
kp ie
ce 6
)
W 3
-X
-Y
G 56
(W or
kp ie
ce 3
)
W 5
-X
-Y
G 58
(W or
kp ie
ce 5
)
W 1
-X
— Y
G 54
(W or
kp ie
ce 1
)
12 5
20 0m
m
17 5
50 m
m
12 5
17 5
50 0m
m
10 0m
m
10 0m
m
50 0m
m
90 0m
m
-X
-Y
0 M
4 3
2 1
20 0m
m
50 75
75
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset
521
(Example 5) Program example when continuously using 48 sets of added workpiece coordinate system offsets. In this example, the offsets for each workpiece are set beforehand in P1 to P48 when 48 workpieces are fixed on a table, as shown in the drawing below.
P8 P7 P1
P2 P3
P4 P5
P6
P9 P10 P16
P15 P14
P13 P12
P11
P24 P23 P17
P18 P19
P20 P21
P22
P25 P26 P32
P31 P30
P29 P28
P27
P40 P39 P33
P34 P35
P36 P37
P38
P41 P42 P48
P47 P46
P45 P44
P43
01000 G28 XYZ ; #100=1 ; G90 ; WHILE [#100LE48]D01 ; G54.1 P#100 ; M98 P1001 ; #100=#100+1 ; END1 ; G28 Z ; G28 XY ; M02 ;
Reference position return Initialize added workpiece coordinate system P No. Absolute value mode Repeat P No. to 48 Set workpiece coordinate system Call sub-program P No. +1 Return to reference position
01001 G43 X-10.Y-10.Z-100.H10.; Contour G01 X-30.; Y-30.; X-10.; Y-10.; G00 G40 Z10.; G98 G81X-20.Y-15.Z-150.R5.F40; Drilling X-25.Y-20.; X-20.Y-25.; X-15.Y-20.; G80 ; M99 ;
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset
522
(Example 6) Program example when the added workpiece coordinate system offsets are transferred
to the standard workpiece coordinate system offsets and used. In this example, the workpiece coordinate system offsets for each workpiece are set beforehand in P1 to P24 when the workpiece is fixed on a rotating table, as shown in the drawing below.
B
X
P19 Z
Y P20
P21 P22 P23
P24
P1 P2
P3
P4 P5 P6
O20000 (Main) G28 XYZB ; G90 ; G00 B0 ; G65 P2001 A1 ; M98 P2002 ; G00 B90. ; G65 P2001 A7 ; M98 P2002 ; G00 B180. ; G65 P2001 A13 ; M98 P2002 ; G00 B270. ; G65 P2001 A19 ; M98 P2002 ; G28 XYB ; M02 ; %
Reference position return Absolute value mode Position table to face 1 Load workpiece offsets Drilling Position table to face 2
Position table to face 3
Position table to face 4
Return to reference position
O2001 Transmission of workpiece offsets #2=5221 ; #3=(#1-1)20+7001 ; #5=0 ; WHILE [#5 LT 6] DO1 ; #6=#6+1 ; #7=#7+1 ;
Leading No. of workpiece coordinate system variables Leading No. of added workpiece coordinate system variables No. of sets counter clear Check No. of sets Set transmission source 1st axis variable No. Set transmission destination 1st axis variable No.
#4=#4+1 ; WHILE [#4 LT 6] DO2 ; #[#6]=#[#7] ; #6=#6+1 ; #7=#7+1 ; #4=#4+1 ; END2 ;
Clear No. of axes counter Check No. of axes Transmit variable data Set transmission source next axis Set transmission destination next axis No. of axes counter +1
#2=#2+20 ; #3=#3+20 ; #5=#5+1 ; END1 ; M99 ; %
Transmission source Set lead of next variable set. Transmission destination Set lead of next variable set. No. of sets counter +1
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset
523
O2002 (Drilling) G54 M98 H100 ; Drilling in G54 coordinate system G55 M98 H100 ; In G55 G56 M98 H100 ; In G56 G57 M98 H100 ; In G57 G58 M98 H100 ; In G58 G59 M98 H100 ; In G59 G28 Z0 ; M99 ; N100 G98 G81 X-20. Y-15. Z-150. R5. F40 ; Fixed cycle for drilling call X-25. Y-20. ; X-20. Y-25. ; X-15. Y-20. ; G80 ; G28 Z ; M99 ; %
14. Coordinates System Setting Functions 14.11 Local Coordinate System Setting ; G52
524
14.11 Local Coordinate System Setting; G52
Function and purpose
The local coordinate systems can be set independently on the G54 through G59 workpiece coordinate systems using the G52 command so that the commanded position serves as the programmed zero point. The G52 command can also be used instead of the G92 command to change the deviation between the zero point in the machining program and the machining workpiece zero point.
Command format
G54 (54 to G59) G52 X__ Y__ Z__ __ ; : Additional axis
Detailed description
(1) The G52 command is valid until a new G52 command is issued, and the tool does not move.
This command comes in handy for employing another coordinate system without changing the zero point positions of the workpiece coordinate systems (G54 to G59).
(2) The local coordinate system offset will be cleared by the dog-type manual reference (zero) position return or reference (zero) position return performed after the power has been switched ON.
(3) The local coordinate system is canceled by (G54 to G59) G52X0 Y0 Z0 0 ;. (4) Coordinate commands in the absolute value (G90) cause the tool to move to the local
coordinate system position.
Reference position
Incremental value
Absolute value Local coordinate systems
Workpiece coordinate system
Workpiece coordinate system offset (Screen setting, G10 L2P_X_Y_
External workpiece coordinate system offset (Screen setting, G10 P0 X_Z_;)
Absolute value
Ln
Ln
Ln (G90) G52X_Y_;
R
M
(G91) G52X_Y_;
Wn(n=1 to 6)
Machine coordinate system (Note) If the program is executed repeatedly, the workpiece coordinate system will deviate each
time. Thus, when the program is completed, the reference position return operation must be commanded.
14. Coordinates System Setting Functions 14.11 Local Coordinate System Setting ; G52
525
(Example 1) Local coordinates for absolute value mode (The local coordinate system offset is not
cumulated)
(1) G28X0Y0 ; (2) G00G90X1. Y1. ; (3) G92X0Y0 ; (4) G00X500Y500 ; (5) G52X1. Y1. ; (6) G00X0Y0 ; (7) G01X500F100 ; (8) Y500 ; (9) G52X0Y0 ; (10) G00X0Y0 ;
Local coordinate system created by (5).
New coordinate system created by (3) Matched with local coordinate system by (9).
Current position
The local coordinate system is created by (5), canceled (9) and matched with the coordinate system for (3).
(3) (2)
(6)
R#1 W1
[W1] (10)
X
(5) (4)
(8) (9)
500 1000 1500 2000 2500 3000
[W1]L1
2500 2000 1500 1000 500
(1)
(7)
(Note) If the program is executed repeatedly, the workpiece coordinate system will deviate each time. Thus, when the program is completed, the reference position return operation must be commanded.
(Example 2) Local coordinates for incremental value mode (The local coordinate system offset is
cumulated.)
(1) G28X0Y0 ; (2) G92X0Y0 ; (3) G91G52X500Y500 ; (4) M98P100 ; (5) G52X1. Y1. ; (6) M98P100 ; (7) G52X-1.5 Y1.5 ; (8) G00G90X0Y0 ; M02 ; (A) O100 ; (B) G90G00X0Y0 ; (C) G01X500 ; (D) Y500 ; (E) G91 ; (F) M99 ;
Local coordinate system created by (5).
Local coordinate system created by (3).
Current position Matched with local coordinate system by (7).
R#1 W1
[W1]L2
X
500 1000 1500 2000 2500 3000
[W1]L1
2500
2000
1500
1000
500 X’
X»
Y» Y’ Y
(1) (2) (3)
(4)
(6)
(B)
(8)
(B) (C)
(D)
(D)
(C)
(Explanation)
The local coordinate system X’Y’ is created at the XY coordinate system (500,500) position by (3). The local coordinate system X»Y» is created at the X’Y’ coordinate system (1000,1000) position by (5). The local coordinate system is created at the X»Y» coordinate system (-1500, -1500) position by (7). In other words, the same occurs as when the local coordinate system and XY coordinate system are matched and the local coordinate system is canceled.
14. Coordinates System Setting Functions 14.11 Local Coordinate System Setting ; G52
526
(Example 3) When used together with workpiece coordinate system
(1) G28X0Y0 ; (2) G00G90G54X0Y0 ; (3) G52X500Y500 ; (4) M98P200 ; (5) G00G90G55X0Y0 ; (6) M98P200 ; (7) G00G90G54X0Y0 ;
~ M02 ; (A) O200 ; (B) G00X0Y0 ; (C) G01X500F100 ; (D) Y500 ; (E) M99 ; %
Workpiece coordinate system (parameter setting value)
G54 G55 X 1000 1000 Y 500 2000
Local coordinate system created by (3)
Current position
500 1000 1500 2000 2500 3000
3000
2500
2000
1500
1000
500
R#1
W1
[W1] L1 G54
X
Y
G55
(B)
(2)
(5) W2
(7)
1
(3)
(B) (D)
(D)
(C)
(C)
(Explanation) The local coordinate system is created at the G54 coordinate system (500,500) position by (3), but the local coordinate system is not created for the G55 coordinate system. During the movement for (7), the axis moves to the G54 local coordinate system’s reference position (zero point). The local coordinate system is canceled by G90G54G52X0Y0;.
14. Coordinates System Setting Functions 14.11 Local Coordinate System Setting ; G52
527
(Example 4) Combination of workpiece coordinate system G54 and multiple local coordinate
systems
(1) G28X0Y0 ; (2) G00G90G54X0Y0 ; (3) M98P300 ; (4) G52X1. Y1. ; (5) M98P300 ; (6) G52X2. Y2. ; (7) M98P300 ; (8) G52X0Y0 ;
~ M02 ; (A) O300 ; (B) G00X0Y0 ; (C) G01X500F100 ; (D) Y500 ; (E) X0Y0 ; (F) M99 ; %
Workpiece coordinate offset (parameter setting value)
G54 X 500 Y 500
Local coordinate system created by (6)
Local coordinate system created by (4)
Current position
(7)
(3)
[W1] L2
500 1000 1500 2000 2500 3000
3000
2500
2000
1500
1000
500
(D)
(C)(E)
(B)
[W1] L1
(8) (2)
R#1
G54
W1
(5)
(Explanation) The local coordinate system is created at the G54 coordinate system (1000,1000) position by (4). The local coordinate system is created at the G54 coordinate system (2000,2000) by (6). The G54 coordinate system and local coordinate system are matched by (8).
14. Coordinates System Setting Functions 14.12 Workpiece Coordinate System Preset; G92.1
528
14.12 Workpiece Coordinate System Preset; G92.1
Function and purpose
(1) This function presets the workpiece coordinate system shifted with the program command
during manual operation to the workpiece coordinate system offset from the machine zero point by the workpiece coordinate offset amount by the program command (G92.1).
(2) The set workpiece coordinate system will be shifted from the machine coordinate system when the following type of operation or program command is executed. When manual interrupt is executed while manual absolute is OFF When movement command is issued in machine lock state When axis is moved with handle interrupt When operation is started with mirror image When local coordinate system is set with G52 When workpiece coordinate system is shifted with G92
This function presets the shifted workpiece coordinate system to the workpiece coordinate system offset from the machine zero point by the workpiece coordinate offset amount. This takes place in the same manner as manual reference position return. Whether to preset the relative coordinates or not can be selected with the parameters.
Command format
G92.1 X0 Y0 Z0 0 ; (G50.3) 0 Additional axis
14. Coordinates System Setting Functions 14.12 Workpiece Coordinate System Preset; G92.1
529
Detailed description
(1) Command the address of the axis to be preset. The axis will not be preset unless commanded.
(2) A program error (P35) will occur if a value other than «0» is commanded.
(3) This can be commanded in the following G code lists. G code list 2 to 7 G code list 1 when the G code changeover parameter (#1267 ext3/bit0 = 1) is set.
(4) Depending on the G code list, the G code will be «G50.3».
(5) When manual operation is carried out when manual absolute is set to OFF, or if the axis is moved with handle interrupt
Manual movement amount
Present position Workpiece coordinate x after preset
X
Y
Workpiece coordinate zero point
X
Y
Preset
W1
W1
W1
M Machine coordinate zero point
Workpiece offset
Present position
Workpiece coordinate zero point
Workpiece coordinate y after preset
If manual operation is carried out when manual absolute is set to OFF, or if the axis is moved with handle interrupt, the workpiece coordinate system will be shifted by the manual movement amount. This function returns the shifted workpiece coordinate zero point W1′ to the original workpiece coordinate zero point W1, and sets the distance from W1 to the present position as the workpiece coordinate system’s present position.
14. Coordinates System Setting Functions 14.12 Workpiece Coordinate System Preset; G92.1
530
(6) When movement command is issued in machine lock state
Movement amount during machine lock
X
Y
X
Y
Preset
W1 W1
Workpiece coordinate system coordinate value Present position
Workpiece coordinate zero point
Workpiece coordinate x after preset
Workpiece coordinate y after preset
Workpiece coordinate zero point
Present position
If the movement command is issued in the machine lock state, the present position will not move, and only the workpiece coordinates will move. This function returns the moved workpiece coordinates to the original present position, and sets the distance from W1 to the present position as the workpiece coordinate system’s present position.
(7) When operation is carried out with mirror image
Mirror image center X
Y
Program command
X
Y
Actual operation
W1 W1
Preset
Present position
Workpiece coordinate zero point
Workpiece coordinate zero point
Present position
Workpiece coordinate x after preset
Workpiece coordinate y after preset
If operation is carried out with mirror image, only the NC internal coordinates are used as the program command coordinates. The other coordinates are the present position coordinates. This function sets the NC internal coordinates as the present position coordinates.
14. Coordinates System Setting Functions 14.12 Workpiece Coordinate System Preset; G92.1
531
(8) Setting local coordinate system with G52
Local coordinate zero point
X
Y
X
Y Local coordinates x
W1
L1
W1
Present position
Workpiece coordinate zero point
Workpiece coordinate x after preset Present position
Workpiece coordinate zero point
Local coordinates y
Workpiece coordinate y after preset
Preset
The local coordinate system is set with the G52 command, and the program commands, etc., are issued with the local coordinate system. With this function, the set local coordinate system is canceled, and the program commands, etc., use the workpiece coordinate system which has W1 as the zero point. The canceled local coordinate system is only the selected workpiece coordinate system.
(9) Shifting the workpiece coordinate system with G92
Workpiece zero point after G92 command
X
Y
X
Y
W1
W1
W1
Present position
Workpiece coordinate zero point
Workpiece coordinate x after preset
Preset
Workpiece coordinate y after preset
Present positionWorkpiece coordinates x
Workpiece coordinates y
Workpiece coordinate zero point
The workpiece coordinate system shifts with the G92 command, and the distance between W1′ and the present position is set as the present position of the workpiece coordinate system. This function returns the shifted workpiece coordinate zero point to W1, and sets the distance from W1 to the present position as the workpiece coordinate system’s present position. This is valid for all workpiece coordinate systems.
14. Coordinates System Setting Functions 14.12 Workpiece Coordinate System Preset; G92.1
532
Example of program
The workpiece coordinate system shifted with G92 is preset with G92.1.
X
Y
X
Y
W1
(1)
W1
(2) (3)
(4) (5)
500
1000
1500
500 1000 1500
500
1000
1500
500 1000 1500
Workpiece zero point after G92 command
Workpiece coordinate zero point Workpiece coordinate zero point
G92.1 command
preset
(Unit: mm) (Unit: mm)
(Example) G28 X0 Y0 ; …………………. (1) G00 G90 X1. Y1. ; ………… (2) G92 X0 Y0 ; …………………. (3) G00 X500 Y500 ;………….. (4) G92.1 X0 Y0 ; ………………. (5)
Precautions
(1) Cancel tool radius compensation, tool length offset and tool position offset before using this
function. If these are not canceled, the workpiece coordinates will be at a position obtained by subtracting the workpiece coordinate offset amount from the machine value. Thus, the compensation vector will be temporarily canceled.
(2) This function cannot be executed while the program is being resumed.
(3) Do not command this function during the scaling, coordinate rotation or program mirror image modes.
A program error (P34) will occur if commanded.
14. Coordinates System Setting Functions 14.13 Coordinate System for Rotary Axis
533
14.13 Coordinate System for Rotary Axis
Function and purpose
The axis designated as the rotary axis with the parameters is controlled with the rotary axis’ coordinate system. The rotary axis includes the rotating type (short-cut valid/invalid) and linear type (workpiece coordinate position linear type, all coordinate position linear type). The workpiece coordinate position range is 0 to 359.999 for the rotating type, and 0 to 99999.999 for the linear type. The machine coordinate position and relative position differ according to the parameters. The rotary axis is commanded with a degree () unit regardless of the inch or metric designation. The rotary axis type can be set with the parameter #8213 rotation axis type for each axis.
Rotary axis
Rotating type rotary axis Linear type rotary axis
Short-cut invalid
Short-cut valid
Workpiece coordinate
position linear type
All-coordinate position
linear type
Linear axis
#8213 setting value 0 1 2 3 —
Workpiece coordinate value
Displayed in the range of 0 to 359.999. Displayed in the range of 0 to 99999.999.
Machine coordinate value/relative position
Displayed in the range of 0 to 359.999. Displayed in the range of 0 to 99999.999.
ABS command
The incremental amount from the end point to the current position is divided by 360, and the axis moves by the remainder amount according to the sign.
Moves with a short-cut to the end point.
In the same manner as the normal linear axis, moves according to the sign by the amount obtained by subtracting the current position from the end point (without rounding up to 360 degrees).
INC command Moves in the direction of the commanded sign by the commanded incremental amount starting at the current position. Until the intermediate point: Depends on the absolute command or the incremental command.
Reference position return From the intermediate point to the reference position:
Returns with movement within 360 degrees.
Moves and returns in the reference position direction by the difference from the intermediate point to the reference position.
14. Coordinates System Setting Functions 14.13 Coordinate System for Rotary Axis
534
Example of operation
Examples of differences in the operation and counter displays according to the type of rotation coordinate are given below. (The workpiece offset is set as 0.) (1) Rotary type (short-cut invalid)
(a) The machine coordinate position, workpiece coordinate position and current position are displayed in the range of 0 to 359.999.
(b) For the absolute command, the axis moves according to the sign by the excessive amount obtained by dividing by 360.
Program Workpiece coordinate
counter
Machine coordinat e counter
G28 C0. N1 G90 C-270. 90.000 90.000 N2 C405. 45.000 45.000 N3 G91 C180 225.000 225.000
90
45
0
N3
N2
N1
(2) Rotation type (short-cut valid)
(a) The machine coordinate position, workpiece coordinate position and current position are displayed in the range of 0 to 359.999.
(b) For the absolute command, the axis rotates to the direction having less amount of movement to the end point.
Program Workpiece coordinate
counter
Machine coordinat e counter
G28 C0. N1 G90 C-270. 90.000 90.000 N2 C405. 45.000 45.000 N3 G91 C180 225.000 225.000
90
45
0
N3 N2
N1
14. Coordinates System Setting Functions 14.13 Coordinate System for Rotary Axis
535
(3) Linear type (workpiece coordinate position linear type)
(a) The coordinate position counter other than the workpiece coordinate position is displayed in the range of 0 to 359.999. The workpiece coordinate position is displayed in the range of 0 to 99999.999.
(b) The movement is the same as the linear axis. (c) During reference position return, the axis moves in the same manner as the linear axis until
the intermediate point. The axis returns with a rotation within 360 from the intermediate point to the reference position.
(d) During absolute position detection, even if the workpiece coordinate position is not within the range of 0 to 359.999, the system will start up in the range of 0 to 359.999 when the power is turned ON again.
Program Workpiece coordinate
counter
Machine coordinate
counter
POSITION counter
G28 C0. N1 G90 C-270.
270.000 90.000 90.000
N2 C405. 405.000 45.000 45.000 N3 G91 C180 585.000 225.000 225.000
When power is turned ON again
Workpiece Machine
90
45
0
N3
N2
N1
225.000 225.000
(4) Linear type (all coordinate values linear type)
(a) The all-coordinate position counter is displayed in the range of 0 to 99999.999. (b) The movement is the same as the linear axis. (c) During reference position return, the axis moves in the same manner as the linear axis until
the intermediate point. The axis rotates by the difference from the intermediate point to the reference position and returns to the reference position.
(d) During absolute position detection, the system starts up at the position where the power was turned OFF when the power is turned ON again.
Program Workpiece coordinate
counter
Machine coordinate
counter
POSITION counter
G28 C0. N1 G90 C-270.
270.000 270.000 270.000
N2 C405. 405.000 405.000 405.000 N3 G91 C180 585.000 585.000 585.000
When power is turned ON again
Workpiece Machine
90
45
0
N3
N2
N1
585.000 585.000
15. Measurement Support Functions 15.1 Automatic Tool Length Measurement; G37
536
15. Measurement Support Functions 15.1 Automatic Tool Length Measurement; G37
Function and purpose
These functions issue the command values from the measuring start position as far as the measurement position, move the tool in the direction of the measurement position, stop the machine once the tool has arrived at the sensor, cause the NC system to calculate automatically the difference between the coordinate values at that time and the coordinate values of the commanded measurement position and provide this difference as the tool offset amount. When offset is already being applied to a tool, it moves the tool toward the measurement position with the offset still applied, and if a further offset amount is generated as a result of the measurement and calculation, it provides further compensation of the present offset amount. If there is one type of offset amount at this time, and the offset amount is distinguished between tool length offset amount and wear offset amount, the wear amount will be automatically compensated.
Command format
G37Z__R__D__F__ ;
G37 : Automatic tool length measurement command Z : Measuring axis address and coordinates of measurement position ….. X, Y, z,
(where, is the additional axis) R : This commands the distance between the measurement position and point where the
movement is to start at the measuring speed. D : This commands the range within which the tool is to stop. F : This commands the measuring feedrate.
When R__, D__ of F__ is omitted, the value set in the parameter is used instead. («TLM» on machining parameter screen) #8004 SPEED (measuring feedrate) : 0 to 1000000 (mm/min) #8005 ZONE r (deceleration range) : 0 to 99999.999 (mm) #8006 ZONE d (measurement range) : 0 to 99999.999 (mm)
15. Measurement Support Functions 15.1 Automatic Tool Length Measurement; G37
537
Example of execution
(1) For new measurement
Tool Reference position (Z0)
To ol
le
ng th
F
R D
D
Measuring device
M ov
em en
t a m
ou nt
b y
to ol
le
ng th
m ea
su re
m en
t
G28 Z0; T01; M06 T02; G90 G00 G43 Z0 H01; G37.1 Z-400 R200 D150 F1; Coordinate value when reached at the measurement position=-300 -300-(-400)=100 Thus, 0+100=100 H01=100.
-100
-200
-300
-400
0
(Note) A new measurement is applied when the current tool length compensation amount is zero.
Thus, length will be compensated whether or not length dimension by tool compensation memory type and length wear are differentiated.
(2) When tool compensation is applied
Tool Reference position (Z0)
F
R
D
D Measuring
device
G28 Z0; T01; M06 T02; G43 G00 Z0 H01; G37.1 Z-400. R200. D50. F10; Coordinate value when reached measurement position=-305 -305-(400)=95 Thus, H01=95.
-100
-200
-300
-400
0
Wear amount
(Note) A measurement for the wear amount is applied when the current tool length compensation
amount is other than zero. Thus, length wear will be compensated if length dimension by tool compensation memory type and length wear are differentiated. If not differentiated, length dimension will be compensated.
15. Measurement Support Functions 15.1 Automatic Tool Length Measurement; G37
538
Detailed description
(1) Operation with G37 command
Speed Rapid traverse rate
Measurement allowable range
Distance
Operation 1 Operation 2 Operation 3
Offset amount
Normal completion Alarm stop (P607) Alarm stop (P607)
D(d) D(d) F(Fp)
R(r)
Measuring position Stop point Sensor output
Or no detection
(2) The sensor signal (measuring position arrival signal) is used in common with the skip signal. (3) The feedrate will be 1mm/min if the F command and parameter measurement speed are 0. (4) An updated offset amount is valid unless it is assigned from the following Z axis (measurement
axis) command of the G37 command. (5) Excluding the delay at the PLC side, the delay and fluctuations in the sensor signal processing
range from 0 to 0.2ms. As a result, the measuring error shown below is caused.
Maximum measuring error (mm) = Measuring speed (mm/min) 1 60 0.2 (ms)
1000
(6) The machine position coordinates at that point in time are ready by sensor signal detection, and the machine will overtravel and stop at a position equivalent to the servo droop.
Maximum overtravel (mm)
= Measuring speed (mm/min) 1 60 1
Position loop gain (s1)
The standard position loop gain is 33 (s1).
15. Measurement Support Functions 15.1 Automatic Tool Length Measurement; G37
539
Precautions
(1) Program error (P600) results if G37 is commanded when the automatic tool length measurement function is not provided.
(2) Program error (P604) results when no axis has been commanded in the G37 block or when two or more axes have been commanded.
(3) Program error (P605) results when the H code is commanded in the G37 block. (4) Program error (P606) results when G43_H is not commanded prior to the G37 block. (5) Program error (P607) results when the sensor signal was input outside the allowable
measuring range or when the sensor signal was not detected even upon arrival at the end point.
(6) When a manual interrupt is applied while the tool is moving at the measuring speed, a return must be made to the position prior to the interrupt and then operation must be resumed.
(7) The data commanded in G37 or the parameter setting data must meet the following conditions:
| Measurement point start point | > R address or parameter r > D address or parameter d (8) When the D address and parameter d in (7) above are zero, operation will be completed
normally only when the commanded measurement point and sensor signal detection point coincide. Otherwise, program error (P607) will results.
(9) When the R and D addresses as well as parameters r and d in (7) above are all zero, program error (P607) will result regardless of whether the sensor signal is present or not after the tool has been positioned at the commanded measurement point.
(10) The automatic tool length measurement command (G37) must be commanded together with the G43H_ command that designates the offset No.
G43H_; G37 Z_ R_ D_ F_;
15. Measurement Support Functions 15.2 Skip Function; G31
540
15.2 Skip Function; G31 Function and purpose
When the skip signal is input externally during linear interpolation based on the G31 command, the machine feed is stopped immediately, the remaining distance is discarded and the command in the following block is executed.
Command format
G31 X__ Y__ Z__ __ F__ ; (where, a is the additional axis) X, Y, Z, : Axis coordinates; they are commanded as absolute or incremental
values according to the G90/G91 modal when commanded. F : Feedrate (mm/min)
Linear interpolation can be executed using this function. If the skip signal is input externally while this command is being executed, the machine will stop, the remaining commands will be canceled and operation will be executed from the next block.
Detailed description
(1) If Ff is assigned as the feedrate in the same block as the G31 command block, command feed
f will apply; if it not assigned, the value set in the parameter «#1174 Skip_F» will serve as the feedrate. In either case, the F modal will not be updated.
(2) The machine will not automatically accelerate and decelerate with the G31 block. The G31 maximum speed will depend on the machine specifications.
(3) Override is invalid with the G31 command and it is fixed at 100%. Dry run is also invalid. The stop conditions (feed hold, interlock, override zero and stroke end) are valid. External deceleration is also valid.
(4) The G31 command is unmodal and so it needs to be commanded each time. (5) If the skip command is input during G31 command start, the G31 command will be completed
immediately. When a skip signal has not been input until the G31 block completion, the G31 command will
also be completed upon completion of the movement commands. (6) When the G31 command is issued during tool radius compensation, program error (P608) will
result. (7) When there is no F command in the G31 command and the parameter speed is also zero,
program error (P603) will result. (8) With machine lock or with a command for the Z axis only with the Z axis cancel switch ON, the
skip signal will be ignored and execution will continue as far as the end of the block.
15. Measurement Support Functions 15.2 Skip Function; G31
541
Execution of G31
G90 G00 X-100000 Y0 ; G31 X-500000 F100 ; G01 Y-100000 ; G31 X0 F100 ; Y-200000 ; G31 X-50000 F100 ; Y-300000 ; X0 ;
-500000 0
-100000
-200000
-300000
-10000
G01
G31
G31
G31
G01 G01
G01 X
W
Y
Detailed description (Readout of skip coordinates)
The coordinate positions for which the skip signal is input are stored in the system variables #5061 (1st axis) to #506n (n-th axis), so these can be used in the user macros.
~ G90 G00 X-100. ;
G31 X-200. F60 ;
#101 = #5061
~
Skip command Skip signal input coordinate values (workpiece coordinate system) are readout to #101.
15. Measurement Support Functions 15.2 Skip Function; G31
542
Detailed description (G31 coasting)
The amount of coasting from when the skip signal is input during the G31 command until the machine stops differs according to the parameter «#1174 skip_F» or F command in G31. The time to start deceleration to a stop after responding to the skip signal is short, so the machine can be stopped precisely with a small coasting amount
0 = F 60 Tp +
F 60 ( t1 t2 ) =
F 60 ( Tp + t1 )
F 60 t2
1 2 0 : Coasting amount (mm) F : G31 skip speed (mm/min.) Tp : Position loop time constant (s) = (position loop gain)1 t1 : Response delay time (s) = (time taken from the detection to the arrival of the skip
signal at the controller via PC) t2 : Response error time (0.001 s)
When G31 is used for calculation, the value calculated from the section indicated by 1 in the above equation can be compensated, however, 2 results in calculation error.
Skip signal input
Stop pattern with skip signal input
Area inside shaded section denotes coasting amount 0
Time (S) Tpt1 t2
F
The relationship between the coasting amount and speed when Tp is 30ms and t1 is 5ms is shown in the following figure.
C oa
st in
g am
ou nt
(m
m )
Average
Feedrate F (mm/min)
Relationship between coasting amount and feedrate (example)
Max. value
Min. value
Tp = 0.03 t1 = 0.0050.050
0.040
0.030
0.020
0.010
0 10 20 30 40 50 60 70
15. Measurement Support Functions 15.2 Skip Function; G31
543
Detailed description (Skip coordinate readout error)
(1) Skip signal input coordinate readout
The coasting amount based on the position loop time constant Tp and cutting feed time constant Ts is not included in the skip signal input coordinate values. Therefore, the workpiece coordinate values applying when the skip signal is input can be read out across the error range in the following formula as the skip signal input coordinate values. However, coasting based on response delay time t1 results in a measurement error and so compensation must be provided.
R ea
do ut
e rro
r (
m )
Readout error of skip signal input coordinates
Readout error of skip input coordinates Readout error with a 60mm/min feedrate is: = 0.001 = 0.001 (mm) Measurement value is within readout error range of 1m.
= t2
+1
0
-1 Measurement value comes within shaded section.
60 Feedrate (mm/min)
60 60
F 60
: Readout error (mm) F : Feedrate (mm/min) t2 : Response error time 0.001 (s)
(2) Readout of other coordinates
The readout coordinate values include the coasting amount. Therefore, when coordinate values are required with skip signal input, reference should be made to the section on the G31 coasting amount and compensation provided. As in the case of (1), the coasting amount based on the delay error time t2 cannot be calculated, and this generates a measuring error.
15. Measurement Support Functions 15.2 Skip Function; G31
544
Examples of compensating for coasting
(1) Compensating for skip signal input coordinates
#110 = Skip feedrate ;
#111 = Response delay time t1 ;
~ G31 X100. F100 ; G04 ; #101 = #5061 ; #102 = #110#111/60 ; #105 = #101#102#103 ;
~
Skip command Machine stop check Skip signal input coordinate readout Coasting based on response delay time Skip signal input coordinates
(2) Compensating for workpiece coordinates
#110 = Skip feedrate ; #111 = Response delay time t1 ; #112 = Position loop time constant Tp ;
~ G31 X100. F100 ; G04 ; #101 = #5061 ; #102 = #110#111/60 ; #103 = #110#112/60 ; #105 = #101#102#103 ;
~
Skip command Machine stop check Skip signal input coordinate readout Coasting based on response delay time Coasting based on position loop time constant Skip signal input coordinates
15. Measurement Support Functions 15.3 Multi-step Skip Function; G31.n, G04
545
15.3 Multi-step Skip Function; G31.n, G04
Function and purpose
The setting of combinations of skip signals to be input enables skipping under various conditions. The actual skip operation is the same as with G31. The G commands which can specify skipping are G31.1, G31.2, G31.3, and G04, and the correspondence between the G commands and skip signals can be set by parameters.
Command format
G31.1 X__ Y__ Z__ __ F__ ;
X Y Z ; Command format axis coordinate word and target coordinates F ; Feedrate (mm/min)
Same with G31.2 and G31.3 ; Ff is not required with G04 As with the G31 command, this command executes linear interpolation and when the preset skip signal conditions have been met, the machine is stopped, the remaining commands are canceled, and the next block is executed.
Detailed description
(1) Feedrate G31.1 set with the parameter corresponds to «#1176 skip1f», G31.2 corresponds to
«#1178 skip2f», and G31.3 corresponds to «#1180 skip3f». (2) A command is skipped if it meets the specified skip signal condition. (3) The G31.n and G04 commands work the same as the G31 command for other than (1) and (2)
above. (4) The feedrates corresponding to the G31.1, G31.2, and G31.3 commands can be set by
parameters. (5) The skip conditions (logical sum of skip signals which have been set) corresponding to the
G31.1, G31.2, G31.3 and G04 commands can be set by parameters. Valid skip signal Parameter
setting 1 2 3 1 2 3 4 5 6 7
(Skip when signal is input.)
15. Measurement Support Functions 15.3 Multi-step Skip Function; G31.n, G04
546
Example of operation
(1) The multi-step skip function enables the following control, thereby improving measurement
accuracy and shortening the time required for measurement. Parameter settings : Skip condition Skip speed G31.1 : 7 20.0mm/min (f1) G31.2 : 3 5.0mm/min (f2) G31.3 : 1 1.0mm/min (f3)
Program example : N10G31.1 X200.0 ; N20G31.2 X40.0 ; N30G31.3 X1.0 ;
Operation
Skip speed
Measurement distance
Input of skip signal 3 Input of skip signal 2 Input of skip signal 1
N10
f
N20
N30
(f1)
(f2)
(f3)
t
(Note 1) If skip signal 1 is input before skip signal 2 in the above operation, N20 is skipped at that point and N30 is also ignored.
(2) If a skip signal with the condition set during G04 (dwell) is input, the remaining dwell time is
canceled and the following block is executed.
15. Measurement Support Functions 15.4 Multi-step Skip Function 2; G31
547
15.4 Multi-step Skip Function 2; G31
Function and purpose
During linear interpolation followed by the skip command (G31), operation can be skipped according to the conditions of the skip signal parameter Pp. Skip signal command P is specified with the external skip signal 1 to 8. If multi-step skip commands are issued simultaneously in different part systems, both part systems perform skip operation simultaneously if the input skip signals are the same, or they perform skip operation separately if the input skip signals are different. The skip operation is the same as with a normal skip command (G31 without P parameter).
1s t p
ar t s
ys te
m
2n d
pa rt
sy st
em
Skip signal 1
Skip signal 1
Z
X2
X1
Same skip signals input in both 1st and 2nd part systems
X1
X2
Z
1s t p
ar t s
ys te
m
2n d
pa rt
sy st
em
Skip signal 1
Skip signal 2
Different skip signals input in 1st and 2nd part systems
If the skip condition specified by the parameter «#1173 dwlskp» (external skip signals 1 to 8 are used for the specification) is met during execution of a dwell command (G04), the remaining dwell time is canceled and the following block is executed. Similarly, if the skip condition is met during revolution dwelling, the remaining revolution is canceled and the following block is executed.
Command format
G31 X__ Z__ __ P__ F__ ; X Z :Command format axis coordinate word and target coordinates P : Skip signal parameter F : Feedrate (mm/min)
15. Measurement Support Functions 15.4 Multi-step Skip Function 2; G31
548
Detailed description
(1) The skip is specified by command speed f. Note that the F modal is not updated. (2) The skip signal is specified by skip signal parameter p. p can range from 1 to 255. If p is
specified outside the range, program error (P35) occurs. Valid skip signal Skip signal
parameter P 8 7 6 5 4 3 2 1 1 2 3 4
253 254 255
(Skip when signal is input.)
(3) The specified skip signal command is a logical sum of the skip signals. (Example)
G31 X100. P5 F100 ;
Operation is skipped if skip signal 1 or 3 is input.
(4) If skip signal parameter Pp is not specified, the skip condition specified by the G31 parameter works. If speed parameter Ff is not specified, the skip speed specified by the G31 parameter works.
Relations between skip and multi-step skip
Skip specifications x o Condition Speed condition Speed G31 X100 ; Without P and F Program error (P601) Skip 1 Parameter
G31 X100 P5 ; Without F Program error (P602) Command
value Parameter
G31 X100 F100 ; Without P Program error (P601) Skip 1 Command
value G31 X100 P5 F100 ; Program error (P602) Command
value Command
value (Note) «Parameter» in the above table indicates that specified with a skip command (G31).
(5) If skip specification is effective and P is specified as an axis address, skip signal parameter P
is given priority and axis address P is ignored. (Example)
G31 P500. F100 ;
This is regarded as a skip signal parameter and program error (P35) results.
(6) Those items other than (1) to (5) are the same with the ordinary skip function (G31 without P).
~ ~ ~ ~
~~ ~~ ~~ ~ ~
~~ ~~ ~~~~
15. Measurement Support Functions 15.5 Speed Change Skip; G31
549
15.5 Speed Change Skip; G31
Function and purpose
When the skip signal is detected during linear interpolation by the skip command (G31), the feedrate is changed.
Command format
G31 X__ Y__ Z__ __ F__ F1=__ … Fn=__ ; (n is the skip signal 1 to
G31 X Y Z F Fn=
: Skip command : Command format axis coordinate word and target coordinates : Feedrate when starting the cutting feed (mm/min) : Feedrate after detecting the skip signal (mm/min)
Fn=0: Movement stop Fn0: Changing the feedrate to fn
F1=Feedrate after inputting the skip signal 1 :
F8=Feedrate after inputting the skip signal 8
Detailed description
(1) When the skip signal for which the feedrate fn0 is commanded, the speed is changed to the
command speed corresponding to the skip signal.
(2) When the skip signal for which the feedrate fn=0 is commanded, the movement is stopped. The acceleration and deceleration time constant at the movement stop does not follow the skip time constant, but the normal G31 skip. After the movement is stopped, the remaining movement commands are canceled and the following block executed.
(3) When the skip signal has not been input until the G31 block completion, the G31 command will be also completed upon completion of the movement command.
(4) When the skip return is valid, the return operation by the skip signal detection is executed after the movement is stopped.
(5) Even if the acceleration and deceleration with the inclination constant G1 (#1201 G1_acc) is valid, the speed change skip will be the operation of the time constant acceleration and deceleration.
(6) When the feedrate command (Fn=fn) is not specified after detecting the skip signal, the normal G31 skip operation will be applied.
15. Measurement Support Functions 15.5 Speed Change Skip; G31
550
(7) If the skip signal is input during the deceleration by the movement command completion, the speed change will be ignored.
f4
f
Speed
Time
f3
f2
0
Skip signal 4
Skip signal 3
f1
Deceleration section by the movement command completion
Skip signal 2 (Speed change) : Invalid Skip signal 1 (Movement stop) : Valid
(8) The skip signal for which the feedrate is not commanded in the program is ignored.
(9) The speed change or the movement stop is performed when detecting the rising edge of the skip signal. Note that if several rising edges are input at 3.5ms intervals or less, they maybe judged the simultaneous input. When they are judged the simultaneous input, the smaller value will be valid.
f4
f
Speed
Time
f3
f2
0
Skip signal 3 + Skip signal 4
f1
Skip signal 1
Time
Skip signal 2
Skip signal 4
Skip signal 3
Skip signal 2
Skip signal 1
15. Measurement Support Functions 15.5 Speed Change Skip; G31
551
(10) If the G31 block is started with the skip signal input, that signal is considered to rise at the same time as the block start.
(11) If the skip signals for changing the speed and for stopping the movement are simultaneously input, the skip signal for stopping the movement will be valid regardless of the size of the number.
(12) If the skip time constant «#2102 skip_tL» is illegal, the «Y51 PARAMETER ERROR 15» will occur, and if the «#2103 skip_t1» is illegal, the «Y51 PARAMETER ERROR 16» will occur.
(13) The items other than (1) to (12) are the same with the G31 command. Example of operation
Example of program
G31 X100. Ff F1=0 F2=f2 F3=f3 F4=f4 ; Operation
f4
f
Speed
Time
f3
f2
0
Skip time constant
Skip signal 4
Skip signal 3
Skip signal 2
Skip signal 1
f1
Position loop time constant (Position loop gain-1)
15. Measurement Support Functions 15.6 Programmable Current Limitation
552
15.6 Programmable Current Limitation
Function and purpose
This function allows the current limit value of the servo axis to be changed to a desired value in the program, and is used for the workpiece stopper, etc. The commanded current limit value is designated with a ratio of the limit current to the rated current.
Command format
G10 L14 Xn ;
L14 : Current limit value setting (+ side/- side) X : Axis address n : Current limit value (%) Setting value: 1 to 999
Precautions and restrictions
(1) If the current limit value is reached when the current limit is valid, the current limit reached
signal is output.
(2) The following two modes can be used as the operation after the current limit is reached. The external signal determines which mode applies.
Normal mode The movement command is executed in the current state. During automatic operation, the movement command is executed to the end, and then the next block is moved to with the droops still accumulated.
Interlock mode The movement command is executed in the current state. During automatic operation, the operation stops at the corresponding block, and the next block is not moved to. During manual operation, the following same direction commands are ignored.
(3) During the current limit, the position droop generated by the current limit can be canceled when the current limit changeover signal of external signals is canceled. (Note that the axis must not be moving.)
(4) The setting range of the current limit value is 1% to 999%. Commands that exceed this range will cause a program error (P35).
(5) If a decimal point is designated with the G10 command, only the integer will be valid. (Example) G10 L14 X10.123 ; The current limit value will be set to 10%.
(6) For the axis name «C», the current limit value cannot be set from the program (G10 command). To set from the program, set the axis address with an incremental axis name, or set the axis name to one other than «C».
15. Measurement Support Functions 15.7 Stroke Check before Travel; G22/G23
553
15.7 Stroke Check before Travel; G22/G23
Function and purpose
By commanding the boundaries from the program with coordinate values on the machine coordinate system, machine entry into that boundary can be prohibited. This can be set only for the three basic axes.
While the normal stored stroke limit stops entry before the prohibited area, this function causes a program error before movement to the block if a command exceeding the valid movement area is issued.
Command format
G22 X__ Y__ Z__ I__ J__ K__;
G23;
Stroke check before travel ON
Stroke check before travel cancel
G22 : Stroke check before travel ON G23 : Stroke check before travel cancel X Y Z : Coordinates of upper point (basic axis name and its coordinate position) I J K : Coordinates of lower point (basic axis name and its coordinate position)
(Note) In the following command format, the basic axes are X, Y and Z. If the basic axis name
differs, command the point 1 coordinate command address with the basic axis name.
Detailed description
(1) The inner side of the boundary commanded with the point 1 coordinate and point 2 coordinate
is the prohibited area. (2) If the command is omitted, «0» will be set for the address. (3) The area designated with this function is different from the area designated with the stored
stroke limit. However, the area enabled by both functions will be the actual valid movement range.
X
Z Y Upper point designated coordinate
Prohibited area
Upper point designated coordinate
(Note) The upper point and lower point are commanded with coordinate on the machine
coordinate system.
15. Measurement Support Functions 15.7 Stroke Check before Travel; G22/G23
554
Precautions and restrictions
(1) This function is valid only when starting the automatic operation. When interrupted with
manual absolute OFF, the prohibited area will also be shifted by the interrupted amount.
(2) An error will occur if the start point or end point is in the prohibited area.
(3) Stroke check will not be carried out for the axes having the same coordinates set for the upper point and the lower point.
(4) The stroke check is carried out with the tool center coordinate values.
(5) If G23X_Y_Z_; etc., is commanded, the command will be interpreted as G23;X_Y_Z;.(2 blocks) Thus, the stroke check before travel will be canceled, then movement will take place with the previous movement modal.
(6) During automatic reference position return, the check will not be carried out from the intermediate point to the reference position. With G29, when moving from the start point to intermediate point, the check will not be carried out.
(7) If there is an address not used in one block, a program error will occur.
(8) When the rotary-type rotation axis is set as a basic axis, the prohibited area will be converted to the range of from 0 to 360 in the same manner as the movement command. If the setting extends over «0», the side containing «0» will be the check area. Example
(a) G22 Z45. K315. : Stroke check area 45. Z 315. (b) G22 Z-115. K-45. : Stroke check area 225. Z 315. (c) G22 Z45. K-45. : Stroke check area 0. Z 45., 315. Z 360.
0 360
-45 315
-115 225
0 360
-45 315
315
4545 (a) (b) (C)
Shaded area: check area
Appendix 1. Program Error
555
Appendix 1. Program Error (The bold characters are the message displayed in the screen.) These alarms occur during automatic operation and the causes of these alarms are mainly program errors which occur for instance when mistakes have been made in the preparation of the machining programs or when programs which conform to the specification have not been prepared.
Error No. Details Remedy
P 10 No. of simultaneous axes over The number of axis addresses commanded in the same block exceeds the specifications.
Divide the alarm block command into two. Check the specifications.
P 11 Illegal axis address The axis address commanded by the program and the axis address set by the parameter do not match.
Revise the axis names in the program.
P 20 Division error An axis command which cannot be divided by the command unit has been issued.
Check the program.
P 29 Not accept command The normal line control command (G40.1, G41.1, G42.1) has been issued during the modal in which the normal line control is not acceptable.
Check the program.
P 30 Parity H error The number of holes per character on the paper tape is even for EIA code and odd for ISO code.
Check the paper tape. Check the tape puncher and tape reader.
P 31 Parity V error The number of characters per block on the paper tape is odd.
Make the number of characters per block on the paper tape even.
Set the parameter parity V selection OFF. P 32 Illegal address
An address not listed in the specifications has been used.
Check and revise the program address. Check and correct the parameters values. Check the specifications.
P 33 Format error The command format in the program is not correct.
Check the program.
Illegal G code A G code not listed in the specifications has been used. An illegal G code was commanded during the coordinate rotation command (G68).
Check and correct the G code address in the program.
P 34
G51.2 or G50.2 was commanded when the rotary tool axis No. (#1501 polyax) was set to «0». G51.2 or G50.2 was commanded when the tool axis was set to the linear axis (#1017 rot «0»).
Check the parameter setting values.
P 35 Setting value range over The setting range for the addresses has been exceeded.
Check the program.
P 36 Program end error «EOR» has been read during tape and memory mode.
Enter the M02 and M30 command at the end of the program.
Enter the M99 command at the end of the subprogram.
Appendix 1. Program Error
556
Error No. Details Remedy
P 37 O, N number zero A zero has been specified for program and sequence Nos.
The program Nos. are designated across a range from 1 to 99999999.
The sequence Nos. are designated across a range from 1 to 99999.
P 38 No spec: Add. Op block skip «/n» has been issued even though there are no optional block skip addition specifications.
Check the specifications.
P 39 No specifications A non-specified G code was specified. The selected operation mode is not used.
Check the specifications.
P 40 Pre-read block error When tool radius compensation is executed there is an error in the pre-read block and so the interference check is disabled.
Reconsider the program.
P 48 Restart pos return incomplete Movement command was executed before executing the block that is restart-searched.
Carry out program restart again. Movement command cannot be executed before executing the block that is restart-searched.
P 49 Invalid restart search Restart search was attempted for the
3-dimensional circular interpolation. Restart search was attempted during the
cylindrical interpolation, polar coordinate interpolation, and tool tip center control.
Reconsider the program. Reconsider the restart search position.
P 50 No spec: Inch/Metric change Inch/Metric changeover (G20/G21) command was issued even though there is no inch/metric conversion specification.
Check the specifications.
P 60 Compensation length over The commanded movement distance is excessive. (Over 231)
Reconsider the axis address command.
P 61 No spec: Unidirectional posit. Unidirectional positioning (G60) was commanded even though there is no unidirectional positioning specification.
Check the specifications.
P 62 No F command No feed rate command has been issued. There is no F command in the cylindrical
interpolation or polar coordinate interpolation immediately after the G95 mode is commanded.
The default movement modal command at power ON is G01. This causes the machine to move without a G01 command if a movement command is issued in the program, and an alarm results. Use an F command to specify the feed rate.
Specify F with a thread lead command. P 63 No spec: High-speed machining
High-speed machining cancel (G5P0) was commanded even though there is no high-speed machining mode specification.
Check the specifications.
P 65 No spec: High speed mode 3 Check the high-speed mode III specifications.
Appendix 1. Program Error
557
Error No. Details Remedy
P 70 Arc end point deviation large There is an error in the arc start and end
points as well as in the arc center. The difference of the involute curve through
the start point and the end point is large. When arc was commanded, one of the two
axes configuring the arc plane was a scaling valid axis.
Check the numerical values of the addresses that specify the start and end points, arc center as well as the radius in the program.
Check the «+» and «-» directions of the address numerical values.
Check the scaling valid axis.
P 71 Arc center error The arc center is not sought during
R-specified circular interpolation. The curvature center of the involute curve
cannot be obtained.
Check the numerical values of the addresses in the program.
Check whether the start point or end point is on the inner side of the base circle for involute interpolation. When carrying out tool radius compensation, check that the start point and end point after compensation are not on the inner side of the base circle for involute interpolation.
Check whether the start point and end point are at an even distance from the center of the base circle for involute interpolation.
P 72 No spec: Herical cutting A helical command has been issued though it is not included in the specifications.
Check the helical specifications. An Axis 3 command was issued by the
circular interpolation command. If there is no helical specification, the linear axis is moved to the next block.
P 73 No spec: Spiral cutting A spiral command was issued despite the fact that such a command does not exist in the specifications.
The G02.1 and G03.1 commands are issued for circular interpolation.
Check the spiral specifications.
P 74 Can’t calculate 3DIM arc The end block was not specified during 3-dimension circular interpolation supplementary modal, and therefore it is not possible to calculate the 3-dimension circular interpolation. Furthermore, it not possible to calculate the 3-dimension circular interpolation due to an interruption during 3-dimension circular interpolation supplementary modal.
Reconsider the program.
P 75 3DIM arc illegal An unusable G code was issued during 3-dimension circular interpolation modal. Or, a 3-dimension circular interpolation command was issued during a modal for which a 3-dimension circular interpolation command cannot be issued.
Reconsider the program.
P 76 No spec: 3DIM arc interpolat G02.4/G03.4 was commanded even though there is no 3-dimension circular interpolation specification.
Check the specifications.
P80 No spec: Hypoth ax interpolat Hypothetical axis interpolation (G07) was commanded even though there is no hypothetical axis interpolation specification.
Check the specifications.
Appendix 1. Program Error
558
Error No. Details Remedy
P 90 No spec: Thread cutting A thread cutting command was issued even though there is no thread cutting command specification.
Check the specifications.
P 91 No spec: Var lead threading Variable lead thread cutting (G34) was commanded even though there is no variable lead thread cutting specification.
Check the specifications.
P 93 Illegal pitch vaule The thread lead (thread pitch) when performing the thread cutting command is incorrect.
Set the correct thread lead command for the thread cutting command.
P100 No spec: Cylindric interpolat A cylindrical interpolation command was issued even though there is no cylindrical interpolation specification.
Check the specifications.
P110 Plane select during figure rot Plane selection (G17/G18/G19) was commanded during figure rotation.
Check the machining program.
P111 Plane selected while coord rot Plane selection commands (G17, G18, G19) were issued during a coordinate rotation command (G68).
After command G68, always issue a plane selection command following a G69 (coordinate rotation cancel) command.
P112 Plane selected while R compen Plane selection commands (G17, G18,
G19) were issued while tool radius compensation (G41, G42) and nose R compensation (G41, G42, G46) commands were being issued.
Plane selection commands were issued after completing nose R compensation commands when there are no further axis movement commands after G40, and compensation has not been cancelled.
Issue plane selection commands after completing (axis movement commands issued after G40 cancel command) tool radius compensation and nose R compensation commands.
P113 Illegal plane select The circular command axis differs from the selected plane.
Issue a circular command after correct plane selection.
P120 No spec: Feed per rotation Feed per rotation (G95) was commanded even though there is no feed per rotation specification.
Check the specifications.
P121 F0 command during arc modal F0 (F 1-digit feed) was commanded during the arc modal (G02/G03).
Check the machining program.
P122 No spec: Auto corner override An auto corner override command (G62) was issued even though there is no auto corner override specification.
Check the specifications. Delete the G62 command from the program.
P123 No spec: High-accuracy control High-accuracy control command was issued even though there is no high-accuracy control specification
Check the specifications.
Appendix 1. Program Error
559
Error No. Details Remedy
P124 No spec: Inverse time feed There is no inverse time option.
Check the specifications.
P125 G93 mode error A G code command that cannot be issued
was issued during G93 mode. G93 command was issued during a modal
for which inverse time feed cannot be performed.
Reconsider the program.
P126 Invalid cmnd in high-accuracy An illegal command was issued during the high-accuracy control mode. A G code group 13 command was issued
during the high-accuracy control mode. Milling, cylindrical interpolation or pole
coordinate interpolation was commanded during the high-accuracy control mode.
Reconsider the program.
P127 No spec: SSS Control The SSS control valid parameter was set to ON although there is no SSS control specification.
Check the specifications. If there is no SSS control specification, set the parameter #8090 SSS ON to 0.
P130 2nd M function code illegal The 2nd miscellaneous function address commanded in the program differs from the address set in the parameters. miscellaneous function.
Check and correct the 2nd miscellaneous function address in the program.
P131 No spec: Cnst surface ctrl G96 A constant surface speed control command (G96) was issued even though there is no specification.
Check the specifications. Change the constant surface speed control
command (G96) to a rotation speed command (G97).
P132 Spindle rotation speed S=0 No spindle rotation speed command has been issued.
Reconsider the program.
P133 Illegal P-No. G96 An invalid constant surface speed control axis has been specified.
Reconsider the parameter specified for the constant surface speed control axis.
P140 No spec: Pos compen cmd The position compensation command (G45 to G48) specifications are not available.
Check the specifications.
P141 Pos compen during rotation Position compensation was commanded during the figure rotation or coordinate rotation command.
Reconsider the program.
P142 Pos compen invalid arc A position compensation invalid arc command was commanded.
Reconsider the program.
Appendix 1. Program Error
560
Error No. Details Remedy
P150 No spec: Nose R compensation Even though there were no tool radius
compensation specifications, tool radius compensation commands (G41 and G42) were issued.
Even though there were no nose R compensation specifications, nose R compensation commands (G41, G42, and G46) were issued.
Check the specifications.
P151 Radius compen during arc mode A compensation command (G40 G41 G42 G43 G44 G46) has been issued in the arc modal (G02 G03).
Issue the linear command (G01) or rapid traverse command (G00) in the compensation command block or cancel block. (Set the modal to linear interpolation.)
P152 No intersection In interference block processing during execution of a tool radius compensation (G41 or G42) or nose R compensation (G41 G42 or G46) command the intersection point after one block is skipped cannot be determined.
Reconsider the program.
P153 Compensation interference An interference error has arisen while the tool radius compensation command (G41 G42) or nose R compensation command (G41 G42 G46) was being executed.
Reconsider the program.
P154 No spec: 3D compensation A three-dimensional compensation command was issued even though there are no three-dimensional compensation specifications.
Check the specifications.
P155 Fixed cyc exec during compen A fixed cycle command has been issued in the radius compensation mode.
The radius compensation mode is established when a fixed cycle command is executed and so the radius compensation cancel command (G40) should be issued.
P156 R compen direction not defined At the start of G46 nose R compensation the compensation direction is undefined if this shift vector is used.
Change the vector to that with which the compensation direction is defined.
Exchange with a tool having a different tip point No.
P157 R compen direction changed During G46 nose R compensation the compensation direction is inverted.
Change the G command to that which allows inversion of the compensation direction (G00 G28 G30 G33 or G53).
Exchange with a tool having a different tip point No.
Turn ON the «#8106 G46 NO REV-ERR» parameter.
P158 Illegal tip point During G46 nose R compensation the tip point is illegal (other than 1 to 8).
Change the tip point No. to a legal one.
Appendix 1. Program Error
561
Error No. Details Remedy
P170 No offset number The compensation No. (DOO TOO HOO) command was not given when the radius compensation (G41 G42 G43 G46) command was issued. Alternatively the compensation No. is larger than the number of sets in the specifications.
Add the compensation No. command to the compensation command block.
Check the number of compensation No. sets a correct it to a compensation No. command within the permitted number of tool compensation sets.
P171 No spec:Comp input by prog G10 Compensation data input by program (G10) was commanded even though there is no specification of compensation data input by program.
Check the specifications.
P172 G10 L number error (G10 L-No. error) The L address command is not correct when the G10 command is issued.
Check the address L-No. of the G10 command and correct the No.
P173 G10 P number error (G10 compensation error) When the G10 command is issued a compensation No. outside the permitted number of sets in the specifications has been commanded for the compensation No. command.
First check the number of compensation sets and then set the address P designation to within the permitted number of sets.
P174 No spec:Comp input by prog G11 Compensation data input by program cancel (G11) was commanded even though there is no specification of compensation data input by program.
Check the specifications.
P177 Tool life count active Registration of tool life management data with G10 was attempted when the used data count valid signal was ON.
The tool life management data cannot be registered when counting the used data. Turn the used data count valid signal OFF.
P178 Tool life data entry over The number of registration groups total number of registered tools or the number of registrations per group exceeded the specifications range.
Review the number of registrations.
P179 Illegal group No. When registering the tool life management
data with G10 the group No. was commanded in duplicate.
A group No. that was not registered was designated during the T 99 command.
An M code command must be issued as a single command but coexists in the same block as that of another M code command.
The M code commands set in the same group exist in the same block.
The group No. cannot be commanded in duplicate. When registering the group data register it in group units.
Correct to the correct group No.
P180 No spec: Drilling cycle A fixed cycle command was issued though there are not fixed cycle (G72 — G89) specifications.
Check the specifications. Correct the program.
Appendix 1. Program Error
562
Error No. Details Remedy
P181 No spindle command (Tap cycle) Spindle rotation speed (S) has not been commanded in synchronous tapping.
Command the spindle rotation speed (S) in synchronous tapping.
When «#8125 Check Scode in G84» is set to «1», enter the S command in the same block where the synchronous tapping command is issued.
P182 Synchronous tap error Connection to the main spindle unit was not
established. The synchronous tapping was attempted
with the spindle not serially connected under the multiple-spindle control I.
Check connection to the main spindle. Check that the main spindle encoder exists. Set 1 to the parameter #3024 (sout).
P183 No pitch/thread number The pitch or thread number command has not been issued in the tap cycle of a fixed cycle for drilling command.
Specify the pitch data and the number of threads by F or E command.
P184 Pitch/thread number error The pitch or the number of threads per inch
is illegal in the tap cycle of the fixed cycle for drilling command.
The pitch is too small for the spindle rotation speed.
The thread number is too large for the spindle rotation speed.
Check the pitch or the number of threads per inch.
P185 No spec: Sync tapping cycle Synchronous tapping cycle (G84/G74) was commanded even though there is no synchronous tapping cycle specification.
Check the specifications.
P186 Illegal S cmnd in synchro tap S command was issued during synchronous tapping modal.
Cancel the synchronous tapping before issuing the S command.
P190 No spec: Turning cycle A lathe cutting cycle command was input although the lathe cutting cycle was undefined in the specification.
Check the specification. Delete the lathe cutting cycle command.
P191 Taper length error In the lathe cutting cycle the specified length of taper section is illegal.
The radius set value in the lathe cycle command must be smaller than the axis shift amount.
P192 Chamfering error Chamfering in the thread cutting cycle is illegal.
Set a chamfering amount not exceeding the cycle.
P200 No spec: MRC cycle The compound type fixed cycle for turning machining I (G70 to G73) was commanded when the compound type fixed cycle for turning machining I specifications were not provided.
Check the specification.
Appendix 1. Program Error
563
Error No. Details Remedy
P201 Program error (MRC) When called with a compound type fixed
cycle for turning machining I command, the subprogram contained at least one of the following commands:
Reference position return command (G27, G28, G29, G30)
Thread cutting (G33, G34) Fixed cycle skip-function (G31, G31.n)
The first move block of the finish shape program in compound type fixed cycle for turning machining I contains an arc command.
Delete the following G codes from this subprogram that is called with the compound type fixed cycle for turning machining I commands (G70 to G73): G27 G28 G29, G30 G31 G33 G34, and fixed cycle G codes.
Remove G2 and G3 from the first move block of the finish shape program in compound type fixed cycle for turning machining I.
P202 Block over (MRC) The number of blocks in the shape program of the compound type fixed cycle for turning machining I is over 50 or 200 (this differs according to the model).
Specify 50 or a less value. The number of blocks in the shape program called by the compound type fixed cycle for turning machining I commands (G70 to G73) must be decreased below 50 or 200 (this differs according to the model).
P203 D cmnd figure error (MRC) The compound type fixed cycle for turning machining I (G70 to G73) shape program could not cut the work normally because it defined an abnormal shape.
Check the compound type fixed cycle for turning machining I (G70 to G73) shape program.
P204 E cmnd fixed cycle error A command value of the compound type fixed cycle for turning machining (G70 to G76) is illegal.
Check the compound type fixed cycle for turning machining (G70 to G76) command value.
P210 No spec: Pattern cycle A compound type fixed cycle for turning machining II (G74 to G76) command was input although it was undefined in the specification.
Check the specification.
P220 No spec: Special fixed cycle No special fixed cycle specifications are available.
Check the specifications.
P221 No. of special fixed holes = 0 A 0 has been specified for the number of holes in special fixed cycle mode.
Reconsider the program.
P222 G36 angle error A G36 command specifies 0 for angle intervals.
Reconsider the program.
P223 G12/G13 radius error The radius value specified with a G12 or G13 command is below the compensation amount.
Reconsider the program.
P224 No spec: Circular (G12/G13) There are no circular cutting specifications.
Check the specifications.
Appendix 1. Program Error
564
Error No. Details Remedy
P230 Subprogram nesting over A subprogram has been called 8 or more
times in succession from the subprogram. The program in the data server contains the
M198 command. The program in the IC card has been called
more than once (the program in the IC card can be called only once at a time).
Check the number of subprogram calls and correct the program so that it does not exceed 8 times.
P231 No sequence No. At subprogram call time the sequence No. set at return from the subprogram or specified by GOTO was not set.
Specify the sequence Nos. in the call block of the subprogram.
P232 No program No. The machining program has not been found
when the machining program is called. The file name of the program registered in
IC card is not corresponding to O No.
Enter the machining program. Check the subprogram storage destination
parameters. Ensure that the external device (including IC
card) that contains the file is mounted. P235 Program editing
Operation was attempted for the file under program editing.
Execute the program again after completion of program editing.
P240 Program editing Operation was attempted for the file under program editing.
Check the specifications.
P241 No variable No. The variable No. commanded is out of the range specified in the specifications.
Check the specifications. Check the program variable No.
P242 = not defined at vrble set The «=» sign has not been commanded when a variable is defined.
Designate the «=» sign in the variable definition of the program.
P243 Can’t use variables An invalid variable has been specified in the left or right side of an operation expression.
Correct the program.
P244 Invalid set date or time Date or time was set earlier than current date or time in the system variables (#3011, #3012) when the credit system was valid.
Date or time cannot be changed. Reconsider the program.
P250 No spec: Figure rotation Figure rotation (M98 I_J_P_H_L_) was commanded even though there is no figure rotation specification.
Check the specifications.
P251 Figure rotation overlapped Figure rotation command was issued during figure rotation.
Check the machining program.
P252 Coord rotate in fig. rotation A coordinate rotation related command (G68, G69) was issued during figure rotation.
Reconsider the program.
P260 No spec: Coordinates rotation Even though there were no coordinate rotation specifications, a coordinate rotation command was issued.
Check the specifications.
Appendix 1. Program Error
565
Error No. Details Remedy
P270 No spec: User macro A macro specification was commanded though there are no such command specifications.
Check the specifications.
P271 No spec: Macro interrupt A macro interruption command has been issued though it is not included in the specifications.
Check the specifications.
P272 NC and macro texts in a block A statement and a macro statement exist together in the same block.
Reconsider the program and place the executable statement and macro statement in separate blocks.
P273 Macro call nesting over The number of macro call nests exceeded the specifications.
Reconsider the program and correct it so that the macro calls do not exceed the limit imposed by the specification.
P275 Macro argument over The number of macro call argument type II sets has exceeded the limit.
Reconsider the program.
P276 Illegal G67 command A G67 command was issued though it was not during the G66 command modal.
Reconsider the program. The G67 command is the call cancel
command and so the G66 command must be designated first before it is issued.
P277 Macro alarm message An alarm command has been issued in #3000.
Refer to the operator messages on the DIAG screen.
Refer to the instruction manual issued by the machine tool builder.
P280 Brackets [ ] nesting over The number of parentheses «[» or «]» which can be commanded in a single block has exceeded five.
Reconsider the program and correct it so the number of «[» or «]» is five or less.
P281 Brackets [ ] not paired The number of «[» and «]» parentheses commanded in a single block does not match.
Reconsider the program and correct it so that «[» and «]» parentheses are paired up properly.
P282 Calculation impossible The arithmetic formula is incorrect.
Reconsider the program and correct the formula.
P283 Divided by zero The denominator of the division is zero.
Reconsider the program and correct it so that the denominator for division in the formula is not zero.
P290 IF sentence error There is an error in the IF conditional GOTO statement.
Reconsider the program.
P291 WHILE sentence error There is an error in the WHILE conditional DO -END statement.
Reconsider the program.
P292 SETVN sentence error There is an error in the SETVN statement when the variable name setting was made.
Reconsider the program. The number of characters in the variable
name of the SETVN statement must be 7 or less.
P293 DO-END nesting over The number of DO-END nesting levels in WHILE conditional DO -END statement has exceeded 27.
Reconsider the program and correct it so that the nesting levels of the DO — END statement does not exceed 27.
Appendix 1. Program Error
566
Error No. Details Remedy
P294 DO and END not paired The DO’s and END’s are not paired off properly.
Reconsider the program and correct it so that the DO’s and END’s are paired off properly.
P295 WHILE/GOTO in tape There is a WHILE or GOTO statement on the tape during tape operation.
During tape operation a program which includes a WHILE or GOTO statement cannot be executed and so the memory operation mode is established instead.
P296 No address (macro) A required address has not been specified in the user macro.
Review the program.
P297 Address-A error The user macro does not use address A as a variable.
Review the program.
P298 G200-G202 cmnd in tape User macro G200 G201 or G202 was specified during tape or MDI mode.
Review the program.
P300 Variable name illegal The variable names have not been commanded properly.
Reconsider the variable names in the program and correct them.
P301 Variable name duplicated The name of the variable has been duplicated.
Correct the program so that the name is not duplicated.
P310 Not use GMSTB macro code G, M, S, T, or B macro code was called during fixed cycle.
Review the program. Review the parameter.
P350 No spec: Scaling command The scaling command (G50, G51) was issued when the scaling specifications were not available.
Check the specifications.
P360 No spec: Program mirror A mirror image (G50.1 or G51.1) command has been issued though the programmable mirror image specifications are not provided.
Check the specifications.
P370 No spec: Facing t-post MR The facing turret mirror image specifications are not provided.
Check the specifications.
P371 Facing t-post MR illegal Mirror image for facing tool posts was commanded to an axis for which external mirror image or parameter mirror image is valid. Mirror image for facing tool posts validating mirror image for a rotary axis was commanded.
Check the program. Check the parameters.
P380 No spec: Corner R/C The corner R/C was issued when the corner R/C specifications were not available.
Check the specifications. Remove the corner chamfering/corner
rounding command from the program.
Appendix 1. Program Error
567
Error No. Details Remedy
P381 No spec: Arc R/C Corner chamfering II /corner rounding II was specified in the arc interpolation block although corner chamfering/corner rounding II is unsupported.
Check the specifications.
P382 No corner movement The block next to corner chamfering/ corner rounding is not a movement command.
Replace the block succeeding the corner chamfering/corner rounding command by G01 command.
P383 Corner movement short In the corner chamfering/corner rounding command the movement distance was shorter than the value in the corner chamfering/corner rounding command.
Make the corner chamfering/corner rounding less than the movement distance since this distance is shorter than the corner chamfering/ corner rounding.
P384 Corner next movement short When the corner chamfering/corner rounding command was input the movement distance in the following block was shorter than the length of the corner chamfering/corner rounding.
Make the corner chamfering/corner rounding less than the movement distance since this distance in the following block is shorter than the corner chamfering/corner rounding.
P385 Corner during G00/G33 A block with corner chamfering/corner rounding was given during G00 or G33 modal.
Recheck the program.
P390 No spec: Geometric A geometric command was issued though there are no geometric specifications.
Check the specifications.
P391 No spec: Geometric arc There are no geometric IB specifications.
Check the specifications.
P392 Angle < 1 degree (GEOMT) The angular difference between the geometric line and line is 1 or less.
Correct the geometric angle.
P393 Inc value in 2nd block (GEOMT) The second geometric block was specified by an incremental value.
Specify this block by an absolute value.
P394 No linear move command (GEOMT) The second geometric block contains no linear command.
Specify the G01 command.
P395 Illegal address (GEOMT) The geometric format is invalid.
Recheck the program.
P396 Plane selected in GEOMT ctrl A plane switching command was executed during geometric command processing.
Execute the plane switching command before geometric command processing.
P397 Arc error (GEOMT) In geometric IB the circular arc end point does not contact or cross the next block start point.
Recheck the geometric circular arc command and the preceding and following commands.
P398 No spec: Geometric1B Although the geometric IB specifications are not included a geometric command is given.
Check the specifications.
Appendix 1. Program Error
568
Error No. Details Remedy
P411 Illegal modal G111 G111 was issued during milling mode. G111 was issued during nose R
compensation mode. G111 was issued during constant surface
speed. G111 was issued during mixed
synchronization control. G111 was issued during fixed cycle. G111 was issued during polar coordinate
interpolation. G111 was issued during cylindrical
interpolation mode.
Before commanding G111, cancel the following commands. Milling mode Nose R compensation Constant surface speed Mixed synchronization control Fixed cycle Polar coordinate interpolation Cylindrical interpolation
P412 P412 No spec: Axis name switch Axis name switch (G111) was issued even though there is no axis name switch (G111) specification.
Check the specifications.
P420 No spec: Para input by program Parameter input by program (G10) was commanded even though there is no specification of parameter input by program.
Check the specifications.
P421 Parameter input error The specified parameter No. or set data is
illegal. An illegal G command address was input in
parameter input mode. A parameter input command was input
during fixed cycle modal or nose R compensation.
G10L50, G10L70, G11 were not commanded in independent blocks.
Check the program.
P430 R-pnt return incomplete A command was issued to move an axis
which has not returned to the reference position away from that reference position.
A command was issued to an axis removal axis.
Execute reference position return manually. The command was issued to an axis for which
axis removal is validated so invalidate axis removal.
P431 No spec: 2,3,4th R-point ret A command for second third or fourth reference position return was issued though there are no such command specifications.
Check the specifications.
P432 No spec: Start position return Start position return (G29) was commanded even though there is no start position return specification.
Check the specifications.
P433 No spec: R-position check Reference position check (G27) was commanded even though there is no reference position check specification.
Check the specifications.
Appendix 1. Program Error
569
Error No. Details Remedy
P434 Compare error One of the axes did not return to the reference position when the reference position check command (G27) was executed.
Check the program.
P435 G27 and M commands in a block An M command was issued simultaneously in the G27 command block.
An M code command cannot be issued in a G27 command block and so the G27 command and M code command must be placed in separate blocks.
P436 G29 and M commands in a block An M command was issued simultaneously in the G29 command block.
An M code command cannot be issued in a G29 command block and so the G29 command and M code command must be placed in separate blocks.
P438
G52 invalid during G54.1 A local coordinate system command was issued during execution of the G54.1 command.
Review the program.
P450 No spec: Chuck barrier The chuck barrier on command (G22) was specified although the chuck barrier was undefined in the specification.
Check the specification.
P451 No spec: Stroke chk bef travel Stroke check before travel (G22/G23) was commanded even though there is no stroke check before travel specification.
Check the specification.
P452 Limit before travel exists An illegal command such as the start or end point of the traveling axis is inside the prohibited area or the axis passes through the prohibited area, was detected when Stroke check before travel (G22) was ON.
Review the coordinate values of the axis address commanded in the program.
P460 Tape I/O error An error has arisen in the tape reader or alternatively in the printer during macro printing.
Check the power and cable of the connected devices.
Check the I/O device parameters.
P461 File I/O error A file of the machining program cannot be read. IC card has not been inserted.
In memory mode, the programs stored in memory may have been destroyed. Output all of the programs and tool data once and format them.
Ensure that the external device (including an IC card, etc) that contains the file is mounted.
Check the parameters for HD operation or IC card operation.
P462 Computer link commu error A communication error occurred during the BTR operation.
«L01 Computer link error» is displayed simultaneously, so remedy the problem according to the error No.
P480 No spec: Milling Milling was commanded when the milling
specifications were not provided. Polar coordinate interpolation was
commanded when the polar coordinate interpolation specifications were not provided.
Check the specification.
Appendix 1. Program Error
570
Error No. Details Remedy
P481 Illegal G code (mill) An illegal G code was used during the
milling mode. An illegal G code was used during
cylindrical interpolation or polar coordinate interpolation.
The G07.1 command was issued during the tool radius compensation.
Check the program.
P482 Illegal axis (mill) A rotary axis was commanded during the
milling mode. Milling was executed even though an illegal
value was set for the milling axis No. Cylindrical interpolation or polar coordinate
interpolation was commanded during mirror image.
Cylindrical interpolation or polar coordinate interpolation was commanded before the tool compensation was completed after the T command.
G07.1 was commanded when cylindrical interpolation was not possible (there is no rotary axis, or external mirror image is ON).
An axis other than a cylindrical coordinate system axis was commanded during cylindrical interpolation.
Check the machining program, parameters and PLC I/F signal.
P484 R-pnt ret incomplete (mill) Movement was commanded to an axis that
had not completed reference position return during the milling mode.
Movement was commanded to an axis that had not completed reference position return during cylindrical interpolation or polar coordinate interpolation.
Carry out manual reference position return.
Appendix 1. Program Error
571
Error No. Details Remedy
P485 Illegal modal (mill) The milling mode was turned ON during
nose R compensation or constant surface speed control.
A T command was issued during the milling mode.
The mode was switched from milling to cutting during tool compensation.
Cylindrical interpolation or polar coordinate interpolation was commanded during the constant surface speed control mode (G96).
The command unacceptable in the cylindrical interpolation was issued.
A T command was issued during the cylindrical interpolation or polar coordinate interpolation mode.
A movement command was issued when the plane was not selected just before or after the G07.1 command.
A plane selection command was issued during the polar coordinate interpolation mode.
Cylindrical interpolation or polar coordinate interpolation was commanded during tool radius compensation.
The G16 plane in which the radius value of a cylinder is 0 was specified.
A cylindrical interpolation or polar coordinate interpolation command was issued during coordinate rotation by program (G68).
Check the program. Before issuing G12.1, issue G40 or G97. Before issuing G12.1, issue a T command. Before issuing G13.1, issue G40. Specify the radius value of a cylinder other
than 0, or specify the X axis’s current value other than 0 before issuing G12.1/G16.
P486 Milling error The milling command was issued during the
mirror image (when parameter or external input is turned ON).
Polar coordinate interpolation, cylindrical interpolation or milling interpolation was commanded during mirror image for facing tool posts.
The start command of the cylindrical interpolation or polar coordinate interpolation was issued during the normal line control.
Check the program.
P511 Synchronization M code error Two or more synchronization M codes were
commanded in the same block. The synchronization M code and «!» code
were commanded in the same block. Synchronization with the M code was
commanded in 3rd part system or more. (Synchronization with the M code is valid only in 1st part system or 2nd part system.)
Check the program.
P550 No spec: G06.2(NURBS) There is no NURBS interpolation option.
Check the specifications.
Appendix 1. Program Error
572
Error No. Details Remedy
P551 G06.2 knot error The knot (k) command value is smaller than the value for the previous block.
Reconsider the program. Specify the knot by monotone increment.
P552 Start point of 1st G06.2 err The block end point immediately before the G06.2 command and the G06.2 first block command value do not match.
Match the G06.2 first block coordinate command value with the previous block end point.
P554 Invld manual interrupt in G6.2 Manual interruption using a block was performed while in G06.2 mode.
Perform for blocks other than G06.2 mode when manually interrupting.
P555 Invalid restart during G06.2 Restart was attempted from the block in G06.2 mode.
Restart from the block other than in G06.2 mode.
P600 No spec: Auto TLM An automatic tool length measurement command (G37) was execute though there are no such command specifications.
Check the specifications.
P601 No spec: Skip A skip command (G31) was issued though there are no such command specifications.
Check the specifications.
P602 No spec: Multi skip A multiple skip command (G31.1 G31.2 or G31.3) was issued though there are no such command specifications.
Check the specifications.
P603 Skip speed 0 The skip speed is 0.
Specify the skip speed.
P604 TLM illegal axis No axis or more than one axis was specified in the automatic tool length measurement block.
Specify only one axis.
P605 T & TLM command in a block The T code is in the same block as the automatic tool length measurement block.
Specify this T code before the block.
P606 T cmnd not found before TLM The T code was not yet specified in automatic tool length measurement.
Specify this T code before the block.
P607 TLM illegal signal Before the area specified by the D command or decelerating area parameter d the measurement position arrival signal went ON. The signal remains OFF to the end.
Check the program.
P608 Skip during radius compen A skip command was specified during radius compensation processing.
Specify a radius compensation cancel (G40) command or remove the skip command.
P610 Illegal parameter The parameter setting is not correct. G114.1 was commanded when the spindle
synchronization with PLC I/F command was selected.
G113 was commanded when the spindle-spindle polygon machining option was OFF and the spindle synchronization with PLC I/F command was selected.
Check whether «#1549 Iv0vR1» to «#1553 Iv0vR5» are set in descending order (in order of large values).
Check whether «#1554 Iv0rd2» to «#1557 Iv0rd5» are set in descending order.
Check and correct «#1514 expLinax» and «#1515 expRotax».
Check the program. Check the parameter.
Appendix 1. Program Error
573
Error No. Details Remedy
P611 No spec: Exponential function Specification for exponential interpolation is not available.
Check the specification.
P612 Exponential function error A movement command for exponential interpolation was issued during mirror image for facing tool posts.
Check the program.
P700 Illegal command value Spindle synchronization was commanded to a spindle that is not connected serially.
Check the program. Check the parameter.
P900 No spec: Normal line control A normal line control command (G40.1, G41.1, G42.1) was issued when the normal line control specifications were not provided.
Check the specifications.
P901 Normal line control axis G92 A coordinate system preset command (G92) was issued to a normal line control axis during normal line control.
Check the program.
P902 Normal line control axis error The normal line control axis was set to a
linear axis. The normal line control axis was set to the
linear type rotary axis II axis. The normal line control axis has not been
set. The normal line control axis was the same
as the plane selection axis.
Correct the normal line control axis.
P903 Plane chg in Normal line ctrl The plane selection command (G17, G18, G19) was issued during normal line control.
Delete the plane selection command (G17, G18, G19) from the program for normal line control.
P920 No spec: 3D coord conv There is no specification for 3-dimensional coordinate conversion.
Check the specifications.
P921 Illegal G code at 3D coord A G code command that cannot be performed was made during 3-dimensional coordinate conversion modal.
Refer to «Mitsubishi CNC 700/70 Series Programming Instruction Manual (Machining Center Series)» for further details of usable G commands.
When the basic specification parameter «#1229 set01/bit3» is ON, turn the parameter OFF or specify the constant surface speed control cancel (G97).
P922 Illegal mode at 3D coord A 3-dimensional coordinate conversion command was issued during a modal for which 3-dimensional coordinate conversion cannot be performed.
Refer to «Mitsubishi CNC 700/70 Series Programming Instruction Manual (Machining Center Series)» for further details of usable G commands.
P923 Illegal addr in 3D coord blk A G code for which G68 to combination could not be performed was specified for the same block.
Refer to «Mitsubishi CNC 700/70 Series Programming Instruction Manual (Machining Center Series)» for further details of usable G commands.
Appendix 1. Program Error
574
Error No. Details Remedy
P930 No spec: Tool axis compen A tool length compensation along the tool axis command was issued even though there is no tool length compensation along the tool axis specification.
Check the specifications.
P931 Executing tool axis compen A G code that cannot be commanded exists during tool length compensation along the tool axis.
Reconsider the program.
P932 Rot axis parameter error There is a mistake in the linear axis name and rotary axis name in the rotary axis configuration parameters.
Set the correct value and reboot.
P940 No spec: Tool tip control There is no tool tip center control specification.
Check the specifications.
P941 Invalid T tip control command A tool tip center control command was issued during a modal for which a tool tip center control command cannot be issued.
Reconsider the program.
P942 Invalid cmnd during T tip ctrl A G code that cannot be commanded was issued during tool tip center control.
Reconsider the program.
P943 Tool posture command illegal In the case of tool tip center control type 1, if the signs at the tool-side rotary axis or table base-side rotary axis start and finish points differ, a tool base-side rotary axis or table workpiece-side rotary axis rotation exists for the same block, and does not pass a singular point. In the case of tool tip center control type 2, the posture vector command is incorrect.
Reconsider the program.
P990 PREPRO error Combining commands that required pre-reading (nose R offset corner chamfering/corner rounding geometric I geometric IB and compound type fixed cycle for turning machining) resulted in eight or more pre-read blocks.
Reduce the number of commands that require pre-reading or delete such commands.
Appendix 2. Order of G Function Command Priority
575
Appendix 2. Order of G Function Command Priority (Command in a separate block when possible)
(Note) Upper level: When commanded in the same block indicates that both commands are executed
simultaneously G Group
Commanded G code
01 G00 to G03
02 G17 to G19
03 G90, G91
05
G94, G95 06
G20, G21 07
G40 to G42
08 G43, G44,
G49
G command commanded last is valid.
Arc and G41, G42 cause error P151
Arc and G43 to G49 cause error P70
G00 to G03.1 Positioning/ interpolation
Group 1 modal is updated
Also possible during arc modal
Tool radius is compensated, and then axes move.
The G49 movement in the arc modal moves with G01
Group 1 modal is updated G04 is
executed
G04 is executed G40 to G42 are ignored
G04 is executed G43 to G49 are ignored G04
Dwell
G09 Exact stop
check
G10 is priority for axis No movement I, J, K rotation input
G10 is used for axis, so the selected plan axis will be the basic axis.
G10 to G11 are executed G40 to G42 are ignored
G10 to G11 are executed G43 to G49 are ignored
G10, G11 Program data
setting
G command commanded last is valid.
G17 to G19 Plane selection
Plane axis changeover during tool radius compensation causes error P112
Appendix 2. Order of G Function Command Priority
576
G Group
Commanded G code
01 G00 to G03
02 G17 to G19
03 G90, G91
05
G94, G95 06
G20, G21 07
G40 to G42
08 G43, G44,
G49
Possible in same block
G20, G21 Inch/metric changeover
G00 to G03.1 modals are updated G27 to G30 are executed
G27 to G30 are executed G40 to G42 are ignored
G27 to G30 are executed G43 to G49 are ignored
G27 to G30 Reference
position compare/ return
Error:P608 G31 to G31.3 Skip Error:P608
G command commanded last is valid.
G33
Thread cutting
G37 is executed G00 to G33 are ignored
G37 is executed G40 to G42 are ignored
G37 is executed G43 to G49 are ignored
G37 Automatic tool
length measurement
Arc and G41, G42 cause error P151
G command commanded last is valid.
G40 to G42 Tool radius
compensation
G41 and G42 in arc modal cause error P151
Plane axis changeover during tool radius compensation causes error P112
Appendix 2. Order of G Function Command Priority
577
G Group
Commanded G code
09 G73 to G89
10 G98, G99
12 G54 to G59
13 G61 to G64
14 G66 to G67
17 G96, G97
19
G50.1 G51.1
Group 1 command is executed Group 9 is canceled
G66 to G67 are executed G00 to G03.1 modals are updated
During the arc command, all axis names become mirror center data Movement with mirror shape
G00 to G03.1 Positioning/ interpolation
G04 is executed G73 to G89 are ignored
G04 is executed Group 12 is changed
G04 is executed G50.1 and G51.1 are ignored
G04 Dwell
G09 Exact stop
check
G10 to G11 are executed G73 to G89 are ignored
G10 is executed G54 to G59 modals are updated
G66 to G67 are executed G10 is ignored
G10 to G11 are executed G50.1 and G51.1 are ignored
G10, G11 Program data
setting
G17 to G19 Plane selection
Appendix 2. Order of G Function Command Priority
578
G Group
Commanded G code
09 G73 to G89
10 G98, G99
12 G54 to G59
13 G61 to G64
14 G66 to G67
17 G96, G97
19
G50.1 G51.1
G20, G21 Inch/metric changeover
G66 to G67 are executed G27 to G30 are ignored
G27 to G30 are executed G50.1 and G51.1 are ignored
G27 to G30 Reference
position compare/ return
G31 to G31.3 Skip
Group 1 command is executed Group 9 is canceled
G66 to G67 are executed G33 modals is updated
G33 Thread cutting
G66 to G67
are executed G37 modals is ignored
G37 is executed G50.1 and G51.1 are ignored
G37 Automatic tool
length measurement
Error:P155 G40 to G42
Tool radius compensation Error:P155
Appendix 2. Order of G Function Command Priority
579
G Group
Commanded G code
01 G00 to G03.1
G33
02 G17 to G19
03 G90, G91
05
G94, G95 06
G20, G21 07
G40 to G42
08 G43, G44,
G49
Arc and G43, G44 cause error P70
G command commanded last is valid.
G43, G44, G49 Length
compensation Arc and G43, G44 cause error P70
G50.1 G51.1
Program mirror image
G52 is executed G40 to G42 are ignored
G52 is executed G43 to G49 are ignored
G52 Local
coordinate system
G53 is executed G40 to G42 are ignored
G53 is executed G40 to G42 are ignored
G53 Machine
coordinate system
G54 to G59 Workpiece coordinate
system
G61 to G64 Mode selection
G65 is executed G00 to G03.1 modals are updated
G65 is executed G43 to G49 modals are updated
G65 Macro call
Appendix 2. Order of G Function Command Priority
580
G Group
Commanded G code
01 G00 to G03.1
G33
02 G17, G19
03 G90, G92
05
G94, G95 06
G20, G21 07
G40 to G42
08 G43, G44
G49
G66 to G67 are executed G00 to G03.1 modals are updated
G66 to G67 are executed G43 to G49 modals are updated
G66 to G67 Macro call
G73 to G89 are canceled G01 to G33 modals are updated
Error:P155 Canned cycle during compensation
G73 to G89 Canned cycle
Error:P155
Use in same block
G90, G91 Absolute value/
incremental value
G92 Coordinate
system setting
G command commanded last is valid.
G94, G95 Synchronous/ asynchronous
G96, G97 Constant
surface speed control
G98, G99 Initial point/ R point return
Appendix 2. Order of G Function Command Priority
581
G Group
Commanded G code
09 G73 to G89
10 G98 to G99
12 G54 to G59
13 G61 to G65
14 G66 to G67
17 G96, G97
19
G50.1 G51.1
G66 to G67 are executed G43 to G49 modals are updated
G43, G44, G49 Length
compensation
G66 to G67 are executed G50.1 G51.1 is ignored
G command commanded last is valid.
G50.1 G51.1
Program mirror image
G52 is executed
G73to G89 are ignored
G52 is executed G50.1 G51.1 is ignored
G52 Local
coordinate system
G53 is
executed G50.1 G51.1 is invalid
G53 Machine
coordinate system
G command commanded last is valid.
G66 to G67 are executed G54 to G59 modals are updated
G54 to G59 Workpiece coordinate
system
G command commanded last is valid.
G61 to G64
Mode selection
G65 is executed
G73to G89 are ignored
Error G65 is executed G50.1 G51.1 is ignored
G65 Macro call
Appendix 2. Order of G Function Command Priority
582
G Group
Commanded G code
09 G73 to G89
10 G98, G99
12 G54 to G59
13 G61 to G67
14 G66 to G67
17 G96, G97
19
G50.1 G51.1
G66 to G67 are executed G73 to G89 are ignored
G66 to G67 are executed G54 to G59 modals are updated
G command commanded last is valid.
G66 to G67 are executed G50.1 G51.1 is ignored
G66 to G67 Macro call
G command commanded last is valid.
G command commanded last is valid.
G66 to G67 are executed G73 to G89 are ignored
All axes become mirror center
G73 to G89 Canned cycle
G90, G91 Absolute value/
incremental value
G92 is executed G73 to G89 are ignored
Note that G92 is priority for axis
G92 Coordinate
system setting
G94, G95 Synchronous/ asynchronous
G command commanded last is valid.
G96, G97 Constant
surface speed control
G command commanded last is valid.
G98, G99 Initial point/R point return
INDEX
X — 1
INDEX
Numbers
2nd, 3rd and 4th Reference (Zero) Position Return; G30 ……………..508 3-dimensional Circular Interpolation; G02.4, G03.4……………………….95 3-dimensional Coordinate Conversion ; G68/69 ………………………….456
A Actual Examples of Using User Macros …………………………………….363 Arithmetic Commands …………………………………………………………….351 ASCII Code Macro …………………………………………………………………307 Automatic Coordinate System Setting ……………………………………….503 Automatic Corner Override; G62 ………………………………………………138 Automatic Tool Length Measurement; G37 ………………………………..536
B Basic Machine Coordinate System Selection; G53………………………501 Basic Machine, Workpiece and Local Coordinate Systems…………..499 Buffer Register ………………………………………………………………………..22
C Calling Subprogram with M198 Commands………………………………..289 Calling Subprogram with M98 and M99 Commands…………………….284 Changing of Compensation No. during Compensation Mode ………..203 Circle Cutting; G12, G13 …………………………………………………………378 Circular Interpolation; G02, G03…………………………………………………44 Constant Lead Thread Cutting ; G33…………………………………………..56 Constant Surface Speed Control ………………………………………………152 Constant Surface Speed Control; G96, G97……………………………….152 Control Axes……………………………………………………………………………..1 Control Commands…………………………………………………………………356 Coordinate Rotation by Program; G68/G69………………………………..446 Coordinate Rotation Input by Parameter; G10…………………………….453 Coordinate System for Rotary Axis……………………………………………533 Coordinate System Setting ;G92 ………………………………………………502 Coordinate Systems and Coordinate Zero Point Symbols ………………..2 Coordinate Words and Control Axes ……………………………………..1, 498 Coordinates System Setting Functions………………………………………498 Corner Chamfering » ,C_ «……………………………………………………….370 Corner Chamfering/Corner Rounding I ………………………………………370 Corner Rounding » ,R_ » ………………………………………………………….372 Cutting Feedrate…………………………………………………………………….107 Cutting Mode ; G64 ………………………………………………………………..143 Cylindrical Interpolation; G07.1…………………………………………………..63
D Data Formats…………………………………………………………………………….7 Deceleration Check ………………………………………………………………..134 Decimal Point Input ………………………………………………………………….28 Diameter Designation of Compensation Amount …………………………214 Drilling Cycle with High-Speed Retract ………………………………………274 Dwell ……………………………………………………………………………………144
E Exact Stop Check Mode; G61 ………………………………………………….134 Exact Stop Check; G09 …………………………………………………………..131 Exponential Function Interpolation; G02.3, G03.3 …………………………78 External Output Commands …………………………………………………….359
F F1-digit Feed …………………………………………………………………………108
Feed Functions …………………………………………………………………….. 107 Feed Per Minute/Feed Per Revolution
(Asynchronous Feed/Synchronous Feed); G94, G95……………… 110 Feedrate Designation and Effects on Control Axes…………………….. 116 Figure Rotation; M98 I_ J_ K_…………………………………………………. 289 Fixed Cycles…………………………………………………………………………. 247
G G Code Lists ………………………………………………………………………….. 18 G Command Mirror Image; G50.1, G51.1 …………………………………. 367 G1 -> G0 Deceleration Check …………………………………………………. 136 G1 -> G1 Deceleration Check …………………………………………………. 137 G41/G42 Commands and I, J, K Designation…………………………….. 194 General Precautions for Tool Radius Compensation…………………… 202 Geometric Command …………………………………………………………….. 374
H Helical Interpolation ; G17 to G19, G02, G03………………………………. 52 High-accuracy Control ; G61.1, G08 ………………………………………… 403 High-accuracy Spline Interpolation ; G61.2 ……………………………….. 439 High-speed High-accuracy Control ; G05, G05.1 ……………………….. 420 High-speed High-accuracy Control I, II……………………………………… 420 High-speed Machining Mode ; G05, G05.1 ……………………………….. 417 High-speed Machining Mode I,II ; G05 P1, G05 P2…………………….. 417 Hypothetical Axis Interpolation; G07 ………………………………………… 105
I Inch Thread Cutting; G33…………………………………………………………. 60 Inch/Metric Command Change; G20, G21 ………………………………….. 26 Index Table Indexing ……………………………………………………………… 149 Indexing Increment……………………………………………………………………. 6 Initial Point and R Point Level Return; G98, G99 ……………………….. 277 Input Buffer ……………………………………………………………………………. 22 Input Command Increment Tenfold ……………………………………………… 5 Input Setting Units…………………………………………………………………….. 3 Inputting the Tool Life Management Data by G10 L3 Command…… 241 Inputting the Tool Life Management Data by G10 L30 Command…. 243 Inputting the Tool Life Management Data; G10, G11 ………………….. 241 Interference Check………………………………………………………………… 207 Interpolation Functions…………………………………………………………….. 33 Interrupts during Tool Radius Compensation …………………………….. 200 Inverse Time Feed; G93…………………………………………………………. 112
L Least Command Increments ………………………………………………………. 3 Linear Angle Command………………………………………………………….. 373 Linear Interpolation; G01………………………………………………………….. 40 Local Coordinate System Setting; G52 …………………………………….. 524
M Machine Zero Point and 2nd, 3rd, 4th Reference Positions …………. 500 Macro Call Command…………………………………………………………….. 298 Macro Interrupt; M96, M97 ……………………………………………………… 381 Measurement Support Functions …………………………………………….. 536 Miscellaneous Functions ………………………………………………………… 146 Miscellaneous Functions (M8-digits BCD)…………………………………. 146 Multiple Spindle Control …………………………………………………………. 157 Multiple Spindle Control II ………………………………………………………. 158 Multi-step Skip Function 2; G31 ………………………………………………. 547 Multi-step Skip Function; G31.n, G04……………………………………….. 545
INDEX
X — 2
N
Normal Line Control ; G40.1/G41.1/G42.1………………………………….392 NURBS Interpolation ………………………………………………………………100
O Optional Block Skip ………………………………………………………………….13 Optional Block Skip Addition ; /n ………………………………………………..14 Optional Block Skip; / ……………………………………………………………….13 Order of G Function Command Priority ……………………………………..575 Other Commands and Operations during
Tool Radius Compensation …………………………………………………185
P Parameter Input by Program; G10, G11…………………………………….380 Parity H/V ……………………………………………………………………………….17 Per-second Dwell ; G04…………………………………………………………..144 Plane Selection; G17, G18, G19 ………………………………………………..42 Polar Coordinate Command ; G16/G15……………………………………….84 Polar Coordinate Interpolation; G12.1, G13.1/G112,G113 ……………..71 Position Command Methods ; G90, G91 ……………………………………..24 Position Commands …………………………………………………………………24 Positioning (Rapid Traverse); G00 ……………………………………………..33 Precautions …………………………………………………………………………..361 Precautions Before Starting Machining ……………………………………….21 Precautions for Inputting the Tool Life Management Data…………….246 Pre-read Buffers ………………………………………………………………………23 Program Error………………………………………………………………………..555 Program Formats …………………………………………………………………….10 Program Support Functions……………………………………………………..247 Program/Sequence/Block Numbers ; O, N …………………………………..16 Programmable Current Limitation……………………………………………..552 Programmed Compensation Input ; G10, G11 ……………………………236
R Rapid Traverse Constant Inclination Acceleration/Deceleration …….120 Rapid Traverse Constant Inclination Multi-step
Acceleration/Deceleration …………………………………………………..122 Rapid Traverse Rate ………………………………………………………………107 Reference (Zero) Position Return; G28, G29 ……………………………..504 Reference Position Check; G27 ……………………………………………….511 R-specified Circular Interpolation; G02, G03 ………………………………..49
S Scaling ; G50/G51 ………………………………………………………………….441 Secondary Miscellaneous Functions (B8-digits, A8 or C8-digits)……148 Setting of Workpiece Coordinates in Fixed Cycle Mode ……………….278 Skip Function; G31…………………………………………………………………540 Special Fixed Cycle; G34, G35, G36, G37.1 ………………………………279 Speed Change Skip; G31………………………………………………………..549 Spindle Clamp Speed Setting; G92 …………………………………………..153 Spindle Functions…………………………………………………………………..151 Spindle Functions (S6-digits Analog)…………………………………………151 Spindle Functions (S8-digits)……………………………………………………151 Spindle/C Axis Control…………………………………………………………….154 Spiral/Conical Interpolation; G02.0/G03.1(Type1), G02/G03(Type2)..90 Spline; G05.1…………………………………………………………………………432 SSS Control…………………………………………………………………………..427 Standard Fixed Cycles; G80 to G89, G73, G74, G75, G76 …………..247 Start of Tool Radius Compensation and Z Axis Cut in Operation …..205 Stroke Check before Travel; G22/G23 ………………………………………553 Subprogram Control; M98, M99, M198………………………………………284
T
Tape Codes……………………………………………………………………………… 7 Tape Memory Format………………………………………………………………. 13 Tapping Mode; G63 ………………………………………………………………. 143 Thread Cutting ……………………………………………………………………….. 56 Three-dimensional Tool Radius Compensation ; G40/G41,G42……. 218 Timing-synchronization between Part Systems………………………….. 495 Tool Center Point Control; G43.4/G43.5 …………………………………… 473 Tool Change Position Return; G30.1 to G30.6 …………………………… 389 Tool Compensation ……………………………………………………………….. 161 Tool Compensation Functions…………………………………………………. 161 Tool Functions (T command) ………………………………………………….. 160 Tool Functions (T8-digit BCD)…………………………………………………. 160 Tool Length Compensation in the Tool Axis Direction ; G43.1/G49.. 168 Tool Length Compensation/Cancel; G43, G44/G49 ……………………. 165 Tool Position Offset; G45 to G48 …………………………………………….. 229 Tool radius Compensation Operation……………………………………….. 176 Tool Radius Compensation; G38, G39/G40/G41,G42…………………. 175 Types of Variables ………………………………………………………………… 313
U Unidirectional Positioning; G60 …………………………………………………. 61 User Macro Commands; G65, G66, G66.1, G67………………………… 297 User Macro Specifications………………………………………………………. 297
V Variable Commands………………………………………………………………. 292 Variables ……………………………………………………………………………… 311
W Workpiece Coordinate Changing during Radius Compensation……. 216 Workpiece Coordinate System Preset; G92.1 ……………………………. 528 Workpiece Coordinate System Setting and Offset ;
G54 to G59 (G54.1) ………………………………………………………….. 512
Revision History
Date of revision Manual No. Revision details
Jul. 2004 IB(NA)1500072-A First edition created.
Dec. 2004 IB(NA)1500072-B Contents were revised to correspond to Mitsubishi CNC700 Series software version A. The following sections are added. 2.2 Input Command Increment Tenfold 2.3 Indexing Increment 6.14 3-Dimensional Circular Interpolation 6.15 NURBS Interpolation 7.5 Inverse time feed 12.3 Changes in the Tool Length Compensation in the Tool Axis Direction 13.3.3 Figure rotation 13.5.3 ASCII Code Macro 13.15 High-speed machining mode 13.19 Program coordinate rotation 13.20 Coordinate rotation by parameter 13.21 3-dimensional coordinate conversion 13.22 Tool center point control 13.23 Synchronizing Operation between Part Systems 14.13 Coordinate System for Rotary Axis The following sections are deleted. 10.1 Spindle functions (S2-digits BCD) 10.7 Spindle synchronization control II 10.8.1 Multiple spindle control I (multiple spindle command) 10.8.2 Multiple spindle control I (spindle selection command) Simple zero point return 16 Machining mode Other contents were added/revised/deleted according to specification.
Jun. 2005 IB(NA)1500072-C Contents were revised to correspond to Mitsubishi CNC700 Series software version B1. The following sections are added. 6.16 Hypothetical axis interpolation ; G07 12.4.9 Diameter designation of compensation amount 12.5 Three-dimensional tool radius compensation ; G40/G41,G42 13.9 Geometric command 15.7 Stroke check before travel; G22/G23 The following sections are deleted. 12.7 Inputting the tool life management data; G10, G11 Appendix 1 Parameter Input by Program N No. Correspondence Table
Sept. 2006 IB(NA)1500072-D Contents were revised to correspond to Mitsubishi CNC700 Series software version D0. Contents were revised to correspond to Mitsubishi CNC70 Series software version A0. The «Section» (reference) was added in «3.7 G Code Lists». The following sections are added. 13.19 High-accuracy spline interpolation Index Mistakes were corrected.
Jun. 2007 IB(NA)1500072-E The following sections are added. 7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration 12.8 Inputting the tool life management data Mistakes were corrected.
Date of revision Manual No. Revision details
Aug.2008 IB(NA)1500072-F Contents were revised to correspond to Mitsubishi CNC700 Series software version F0. The following sections are added. 3.4.2 Optional Block Skip Addition 12.4.10 Workpiece Coordinate Changing During Radius Compensation 13.1.2 Drilling Cycle with High-Speed Retract Mistakes are corrected.
Global service network
NORTH AMERICA FA Center EUROPEAN FA Center
ASEAN FA Center
CHINA FA Center
TAIWAN FA Center
HONG KONG FA Center
KOREAN FA Center
North America FA Center (MITSUBISHI ELECTRIC AUTOMATION INC.)
Illinois CNC Service Center 500 CORPORATE WOODS PARKWAY, VERNON HILLS, IL. 60061, U.S.A. TEL: +1-847-478-2500 (Se FAX: +1-847-478-2650 (Se California CNC Service Center 5665 PLAZA DRIVE, CYPRESS, CA. 90630, U.S.A. TEL: +1-714-220-4796 FAX: +1-714-229-3818 Georgia CNC Service Center 2810 PREMIERE PARKWAY SUITE 400, DULUTH, GA., 30097, U.S.A. TEL: +1-678-258-4500 FAX: +1-678-258-4519 New Jersey CNC Service Center 200 COTTONTAIL LANE SOMERSET, NJ. 08873, U.S.A. TEL: +1-732-560-4500 FAX: +1-732-560-4531 Michigan CNC Service Satellite 2545 38TH STREET, ALLEGAN, MI., 49010, U.S.A. TEL: +1-847-478-2500 FAX: +1-269-673-4092 Ohio CNC Service Satellite 62 W. 500 S., ANDERSON, IN., 46013, U.S.A. TEL: +1-847-478-2608 FAX: +1-847-478-2690 Texas CNC Service Satellite 1000, NOLEN DRIVE SUITE 200, GRAPEVINE, TX. 76051, U.S.A. TEL: +1-817-251-7468 FAX: +1-817-416-1439 Canada CNC Service Center 4299 14TH AVENUE MARKHAM, ON. L3R OJ2, CANADA TEL: +1-905-475-7728 FAX: +1-905-475-7935 Mexico CNC Service Center MARIANO ESCOBEDO 69 TLALNEPANTLA, 54030 EDO. DE MEXICO TEL: +52-55-9171-7662 FAX: +52-55-9171-7698 Monterrey CNC Service Satellite ARGENTINA 3900, FRACC. LAS TORRES, MONTERREY, N.L., 64720, MEXICO TEL: +52-81-8365-4171 FAX: +52-81-8365-4171 Brazil MITSUBISHI CNC Agent Service Center (AUTOMOTION IND. COM. IMP. E EXP. LTDA.) ACESSO JOSE SARTORELLI, KM 2.1 18550-000 BOITUVA SP, BRAZIL TEL: +55-15-3363-9900 FAX: +55-15-3363-9911
European FA Center (MITSUBISHI ELECTRIC EUROPE B.V.)
Germany CNC Service Center GOTHAER STRASSE 8, 40880 RATINGEN, GERMANY TEL: +49-2102-486-0 FAX:+49-2102486-591 South Germany CNC Service Center KURZE STRASSE. 40, 70794 FILDERSTADT-BONLANDEN, GERMANY TEL: +49-711-3270-010 FAX: +49-711-3270-0141 France CNC Service Center 25, BOULEVARD DES BOUVETS, 92741 NANTERRE CEDEX FRANCE TEL: +33-1-41-02-83-13 FAX: +33-1-49-01-07-25 Lyon CNC Service Satellite U.K CNC Service Center TRAVELLERS LANE, HATFIELD, HERTFORDSHIRE, AL10 8XB, U.K. TEL: +44-1707-282-846 FAX:-44-1707-278-992 Italy CNC Service Center VIALE COLLEONI 7 — PALAZZO SIRIO, CENTRO DIREZIONALE COLLEONI, 20041 AGRATE BRIANZA — (MI), ITALY TEL: +39-039-60531-342 FAX: +39-039-6053-206 Spain CNC Service Satellite CTRA. DE RUBI, 76-80 -APDO.420 08190 SAINT CUGAT DEL VALLES, BARCELONA SPAIN TEL: +34-935-65-2236 FAX: Turkey MITSUBISHI CNC Agent Service Center (GENEL TEKNIK SISTEMLER LTD. STI.) DARULACEZE CAD. FAMAS IS MERKEZI A BLOCK NO.43 KAT2 80270 OKMEYDANI ISTANBUL, TURKEY TEL: +90-212-320-1640 FAX: +90-212-320-1649 Poland MITSUBISHI CNC Agent Service Center (MPL Technology Sp. z. o. o) UL SLICZNA 34, 31-444 KRAKOW, POLAND TEL: +48-12-632-28-85 FAX: Wroclaw MITSUBISHI CNC Agent Service Satellite (MPL Technology Sp. z. o. o) UL KOBIERZYCKA 23, 52-315 WROCLAW, POLAND TEL: +48-71-333-77-53 FAX: +48-71-333-77-53 Czech MITSUBISHI CNC Agent Service Center (AUTOCONT CONTROL SYSTEM S.R.O. ) NEMOCNICNI 12, 702 00 OSTRAVA 2 CZECH REPUBLIC TEL: +420-596-152-426 FAX: +420-596-152-112
ASEAN FA Center (MITSUBISHI ELECTRIC ASIA PTE. LTD.) Singapore CNC Service Center 307 ALEXANDRA ROAD #05-01/02 MITSUBISHI ELECTRIC BUILDING SINGAPORE 159943 TEL: +65-6473-2308 FAX: +65-6476-7439 Thailand MITSUBISHI CNC Agent Service Center (F. A. TECH CO., LTD) 898/19,20,21,22 S.V. CITY BUILDING OFFICE TOWER 1 FLOOR 12,14 RAMA III RD BANGPONGPANG, YANNAWA, BANGKOK 10120. THAILAND TEL: +66-2-682-6522 FAX: +66-2-682-6020 Malaysia MITSUBISHI CNC Agent Service Center (FLEXIBLE AUTOMATION SYSTEM SDN. BHD.) 60, JALAN USJ 10/1B 47620 UEP SUBANG JAYA SELANGOR DARUL EHSAN MALAYSIA TEL: +60-3-5631-7605 FAX: +60-3-5631-7636 JOHOR MITSUBISHI CNC Agent Service Satellite (FLEXIBLE AUTOMATION SYSTEM SDN. BHD.) NO. 16, JALAN SHAHBANDAR 1, TAMAN UNGKU TUN AMINAH, 81300 SKUDAI, JOHOR MALAYSIA TEL: +60-7-557-8218 FAX: +60-7-557-3404 Indonesia MITSUBISHI CNC Agent Service Center (PT. AUTOTEKNINDO SUMBER MAKMUR) WISMA NUSANTARA 14TH FLOOR JL. M.H. THAMRIN 59, JAKARTA 10350 INDONESIA TEL: +62-21-3917-144 FAX: +62-21-3917-164 India MITSUBISHI CNC Agent Service Center (MESSUNG SALES & SERVICES PVT. LTD.) B-36FF, PAVANA INDUSTRIAL PREMISES M.I.D.C., BHOASRI PUNE 411026, INDIA TEL: +91-20-2711-9484 FAX: +91-20-2712-8115 BANGALORE MITSUBISHI CNC Agent Service Satellite (MESSUNG SALES & SERVICES PVT. LTD.) S 615, 6TH FLOOR, MANIPAL CENTER, BANGALORE 560001, INDIA TEL: +91-80-509-2119 FAX: +91-80-532-0480 Delhi MITSUBISHI CNC Agent Parts Center (MESSUNG SALES & SERVICES PVT. LTD.) 1197, SECTOR 15 PART-2, OFF DELHI-JAIPUR HIGHWAY BEHIND 32ND MILESTONE GURGAON 122001, INDIA TEL: +91-98-1024-8895 FAX: Philippines MITSUBISHI CNC Agent Service Center (FLEXIBLE AUTOMATION SYSTEM CORPORATION) UNIT No.411, ALABAMG CORPORATE CENTER KM 25. WEST SERVICE ROAD SOUTH SUPERHIGHWAY, ALABAMG MUNTINLUPA METRO MANILA, PHILIPPINES 1771 TEL: +63-2-807-2416 FAX: +63-2-807-2417 Vietnam MITSUBISHI CNC Agent Service Center (SA GIANG TECHNO CO., LTD) 47-49 HOANG SA ST. DAKAO WARD, DIST.1 HO CHI MINH CITY, VIETNAM TEL: +84-8-910-4763 FAX: +84-8-910-2593
China FA Center (MITSUBISHI ELECTRIC AUTOMATION (SHANGHAI) LTD.)
China CNC Service Center 2/F., BLOCK 5 BLDG.AUTOMATION INSTRUMENTATION PLAZA, 103 CAOBAO RD. SHANGHAI 200233, CHINA TEL: +86-21-6120-0808 FAX: +86-21-6494-0178 Shenyang CNC Service Center TEL: +86-24-2397-0184 FAX: +86-24-2397-0185 Beijing CNC Service Satellite 9/F, OFFICE TOWER1, HENDERSON CENTER, 18 JIANGUOMENNEI DAJIE, DONGCHENG DISTRICT, BEIJING 100005, CHINA TEL: +86-10-6518-8830 FAX: +86-10-6518-8030 China MITSUBISHI CNC Agent Service Center (BEIJING JIAYOU HIGHTECH TECHNOLOGY DEVELOPMENT CO.) RM 709, HIGH TECHNOLOGY BUILDING NO.229 NORTH SI HUAN ZHONG ROAD, HAIDIAN DISTRICT , BEIJING 100083, CHINA TEL: +86-10-8288-3030 FAX: +86-10-6518-8030 Tianjin CNC Service Satellite RM909, TAIHONG TOWER, NO220 SHIZILIN STREET, HEBEI DISTRICT, TIANJIN, CHINA 300143 TEL: -86-22-2653-9090 FAX: +86-22-2635-9050 Shenzhen CNC Service Satellite RM02, UNIT A, 13/F, TIANAN NATIONAL TOWER, RENMING SOUTH ROAD, SHENZHEN, CHINA 518005 TEL: +86-755-2515-6691 FAX: +86-755-8218-4776 Changchun Service Satellite TEL: +86-431-50214546 FAX: +86-431-5021690 Hong Kong CNC Service Center UNIT A, 25/F RYODEN INDUSTRIAL CENTRE, 26-38 TA CHUEN PING STREET, KWAI CHUNG, NEW TERRITORIES, HONG KONG TEL: +852-2619-8588 FAX: +852-2784-1323
Taiwan FA Center (MITSUBISHI ELECTRIC TAIWAN CO., LTD.) Taichung CNC Service Center NO.8-1, GONG YEH 16TH RD., TAICHUNG INDUSTIAL PARK TAICHUNG CITY, TAIWAN R.O.C. TEL: +886-4-2359-0688 FAX: +886-4-2359-0689 Taipei CNC Service Satellite TEL: +886-4-2359-0688 FAX: +886-4-2359-0689 Tainan CNC Service Satellite TEL: +886-4-2359-0688 FAX: +886-4-2359-0689
Korean FA Center (MITSUBISHI ELECTRIC AUTOMATION KOREA CO., LTD.)
Korea CNC Service Center 1480-6, GAYANG-DONG, GANGSEO-GU SEOUL 157-200, KOREA TEL: +82-2-3660-9631 FAX: +82-2-3664-8668
Notice
Every effort has been made to keep up with software and hardware revisions in the contents described in this manual. However, please understand that in some unavoidable cases simultaneous revision is not possible. Please contact your Mit
Manualsnet FAQs
If you want to find out how the M70 Mitsubishi works, you can view and download the Mitsubishi M70 Machining Center System Programming Manual on the Manualsnet website.
Yes, we have the Programming Manual for Mitsubishi M70 as well as other Mitsubishi manuals. All you need to do is to use our search bar and find the user manual that you are looking for.
The Programming Manual should include all the details that are needed to use a Mitsubishi M70. Full manuals and user guide PDFs can be downloaded from Manualsnet.com.
The best way to navigate the Mitsubishi M70 Machining Center System Programming Manual is by checking the Table of Contents at the top of the page where available. This allows you to navigate a manual by jumping to the section you are looking for.
This Mitsubishi M70 Machining Center System Programming Manual consists of sections like Table of Contents, to name a few. For easier navigation, use the Table of Contents in the upper left corner.
You can download Mitsubishi M70 Machining Center System Programming Manual free of charge simply by clicking the “download” button in the upper right corner of any manuals page. This feature allows you to download any manual in a couple of seconds and is generally in PDF format. You can also save a manual for later by adding it to your saved documents in the user profile.
To be able to print Mitsubishi M70 Machining Center System Programming Manual, simply download the document to your computer. Once downloaded, open the PDF file and print the Mitsubishi M70 Machining Center System Programming Manual as you would any other document. This can usually be achieved by clicking on “File” and then “Print” from the menu bar.
CNC Manual/Mitsubishi CNC/Mitsubishi M700 M70 Series
Instruction Manual and User Guide for Mitsubishi M700 M70 Series. We have 8 Mitsubishi M700 M70 Series manuals for free PDF download.
БИЗНЕС ПАРТНЁР
ТЕХНОЛОГИЯ МЕЖДУНАРОДНЫХ КОММУНИКАЦИЙ
-
+86 13804257830 -
+7 (977) 377-16-01 -
tmk-machine@mail.ru
МЕТАЛЛООБРАБАТЫВАЮЩЕЕ ОБОРУДОВАНИЕ
НЕПОСРЕДСТВЕННО ОТ ПРОИЗВОДИТЕЛЯ.
ГАРАНТИЙНОЕ И ПОСТГАРАНТИЙНОЕ ОБСЛУЖИВАНИЕ.
СКЛАД ОРИГИНАЛЬНЫХ
ЗАПЧАСТЕЙ.
-
+86 (0411) 83642729 -
+86 (0411) 83639033
MITSUBISHI
М70
Программирование
NAVI LATHE
MITSUBISHI
М70
Программирование
NAVI MILL
MITSUBISHI
Руководство по програм-мированию
ПОДРОБНЕЕ
ПОДРОБНЕЕ
ПОДРОБНЕЕ
MITSUBISHI
М700
Руководство по програм-мированию
версия L
MITSUBISHI
М700
Программирование
NAVI MILL
MITSUBISHI
М700
Программирование
NAVI LATHE
ПОДРОБНЕЕ
ПОДРОБНЕЕ
ПОДРОБНЕЕ
MITSUBISHI
М700/70
Руководство по программированию
Токарный вариант
MITSUBISHI
М700
Руководство по програм-мированию
версия М
MITSUBISHI
М700
Инструкция по эксплуатации
ПОДРОБНЕЕ
ПОДРОБНЕЕ
ПОДРОБНЕЕ
ОТПРАВИТЬ СООБЩЕНИЕ
С условием ознакомлен
3+4=
С условием ознакомлен
3+4=
Контакты:
БИЗНЕС ПАРТНЁР
Невозможного не существует
-
+86 (0411) 83642729 -
+ 86 13804257830 -
+7 (977) 377 16-00 -
+7 (977) 377 16-01 -
tmk-machine@mail.ru -
Китай г. Далянь р-он Сиган
-
Contents
-
Table of Contents
-
Bookmarks
Quick Links
Related Manuals for Mitsubishi Electric M700V Series
Summary of Contents for Mitsubishi Electric M700V Series
-
Page 3
MELDAS is a registered trademark of Mitsubishi Electric Corporation. Other company and product names that appear in this manual are trademarks or registered trademarks of the respective companies. -
Page 5
Introduction This manual is a guide for using the MITSUBISHI CNC M700V Series. Programming for M2/M0 format is described in this manual, so read this manual thoroughly before starting programming. Thoroughly study the «Precautions for Safety» on the following page to ensure safe use of this NC unit. -
Page 7: Precautions For Safety
Precautions for Safety Always read the specifications issued by the machine maker, this manual, related manuals and attached documents before installation, operation, programming, maintenance or inspection to ensure correct use. Understand this numerical controller, safety items and cautions before using the unit. This manual ranks the safety precautions into «DANGER», «WARNING»…
-
Page 8
CAUTION 2. Items related to operation Before starting actual machining, always carry out dry operation to confirm the machining program, tool compensation amount and workpiece offset amount, etc. If the workpiece coordinate system offset amount is changed during single block stop, the new setting will be valid from the next block. -
Page 9: Table Of Contents
Contents 1. Control Axes……………………..1 1.1 Coordinate Words and Control Axis………………1 1.2 Coordinate Systems and Coordinate Zero Point Symbols…………2 2. Least Command Increments ………………….3 2.1 Input Setting Units……………………3 2.2 Input Command Increment Tenfold………………5 2.3 Indexing Increment……………………6 3. Data Formats ……………………..7 3.1 Tape Codes……………………..7 3.2 Program Formats ……………………10 3.3 Tape Memory Format………………….13 3.4 Optional Block Skip …………………..13…
-
Page 10
7.5 Inverse Time Feed; G93 …………………112 7.6 Feedrate Designation and Effects on Control Axes …………116 7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration ………120 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration ……122 7.9 Exact Stop Check; G09…………………..131 7.10 Exact Stop Check Mode; G61……………….134 7.11 Deceleration Check………………….134 7.11.1 G1 ->… -
Page 11
13. Program Support Functions ………………..248 13.1 Fixed Cycles……………………248 13.1.1 Standard Fixed Cycles; G80 to G89, G73, G74, G75, G76 ……..248 13.1.2 Drilling Cycle with High-Speed Retract ……………276 13.1.3 Initial Point and R Point Level Return; G98, G99…………279 13.1.4 Setting of Workpiece Coordinates in Fixed Cycle Mode……….281 13.2 Special Fixed Cycle;… -
Page 12
14.5 Coordinate System Setting; G92………………509 14.6 Automatic Coordinate System Setting …………….510 14.7 Reference (Zero) Position Return; G28, G29…………..511 14.8 2nd, 3rd and 4th Reference (Zero) Position Return; G30 ……….515 14.9 Reference Position Check; G27………………518 14.10 Workpiece Coordinate System Setting and Offset ; G54 to G59 (G54.1) …….519 14.11 Local Coordinate System Setting;… -
Page 13: Control Axes
1. Control Axes 1.1 Coordinate Words and Control Axis 1. Control Axes 1.1 Coordinate Words and Control Axis Function and purpose In the standard specifications, there are 3 control axes, but, by adding an additional axis, up to 4 axes can be controlled. The designation of the processing direction responds to those axes and uses a coordinate word made up of alphabet characters that have been decided beforehand.
-
Page 14: Coordinate Systems And Coordinate Zero Point Symbols
1. Control Axes 1.2 Coordinate Systems and Coordinate Zero Point Symbols 1.2 Coordinate Systems and Coordinate Zero Point Symbols Function and purpose Reference position Machine coordinate zero point Workpiece coordinate zero points (G54 — G59) Machine zero point Basic machine coordinate system 1st reference Workpiece Workpiece…
-
Page 15: Least Command Increments
2. Least Command Increments 2.1 Input Setting Units 2. Least Command Increments 2.1 Input Setting Units Function and purpose The input setting units are, as with the compensation amounts, the units of setting data used in common for all axes. The command units are the movement amounts in the program which are commanded with MDI inputs or command tape.
-
Page 16
2. Least Command Increments 2.1 Input Setting Units Detailed description (1) Units of various data These input setting units determine the parameter setting unit, program command unit and the external interface unit for the PLC axis and handle pulse, etc. The following rules show how the unit of each data changes when the input setting unit is changed. -
Page 17: Input Command Increment Tenfold
2. Least Command Increments 2.2 Input Command Increment Tenfold 2.2 Input Command Increment Tenfold Function and purpose The program’s command increment can be multiplied by an arbitrary scale with the parameter designation. This function is valid when a decimal point is not used for the command increment. The scale is set with the parameters.
-
Page 18: Indexing Increment
2. Least Command Increments 2.3 Indexing Increment 2.3 Indexing Increment Function and purpose This function limits the command value for the rotary axis. This can be used for indexing the rotary table, etc. It is possible to cause a program error with a program command other than an indexing increment (parameter setting value).
-
Page 19: Data Formats
3. Data Formats 3.1 Tape Codes 3. Data Formats 3.1 Tape Codes Function and purpose The tape command codes used for this controller are combinations of alphabet letters (A, B, C, … Z), numbers (0, 1, 2 … 9) and signs (+, -, / …). These alphabet letters, numbers and signs are referred to as characters.
-
Page 20
3. Data Formats 3.1 Tape Codes (2) Control out, control in All data between control out «(» and control in «)» or «;» , from «0» to «;» (when label L) are ignored, although these data appear on the setting and display unit. Consequently, the command tape name, No. -
Page 21
3. Data Formats 3.1 Tape Codes ISO code (R-840) Feed holes 8 7 6 5 4 3 2 1 Channel No. • •• • • • •• • • •• •• • • •• • • •• • • • ••… -
Page 22: Program Formats
3. Data Formats 3.2 Program Formats 3.2 Program Formats Function and purpose The prescribed arrangement used when assigning control information to the controller is known as the program format, and the format used with this controller is called the «word address format». Detailed description (1) Word and address A word is a collection of characters arranged in a specific sequence.
-
Page 23
3. Data Formats 3.2 Program Formats <Brief summary of format details> Rotary axis Rotary axis Metric command Inch command (Metric command) (Inch command) ← ← ← Program No. L(O)8 ← ← ← Sequence No. ← ← ← Preparatory function G3/G21 0.001(°) mm/ X+53 Y+53 Z+53 α+53 X+44 Y+44 Z+44 α+44… -
Page 24
3. Data Formats 3.2 Program Formats (Note 4) The description of the brief summary is explained below: Example 1 : L(O)8 :8-digit program No. Example 2 : G21 :Dimension G is 2 digits to the left of the decimal point, and 1 digit to the right. Example 3 : X+53 :Dimension X uses + or — sign and represents 5 digits to the left of the decimal point and 3 digits to the right. -
Page 25: Tape Memory Format
3. Data Formats 3.3 Tape Memory Format 3.3 Tape Memory Format Function and purpose (1) Storage tape and significant sections The others are about from the current tape position to the EOB. Accordingly, under normal conditions, operate the tape memory after resetting. The significant codes listed in «Table of tape codes»…
-
Page 26: Optional Block Skip Addition ; /N
3. Data Formats 3.4 Optional Block Skip 3.4.2 Optional Block Skip Addition ; /n Function and purpose Whether the block with «/n (n:1 to 9)» (slash) is executed during automatic operation and searching is selected. By using the machining program with «/n» code, different parts can be machined by the same program.
-
Page 27
3. Data Formats 3.4 Optional Block Skip (2) When two or more «/n» codes are commanded to the head of the same block, the block is ignored if either of the optional block skip signal corresponding to the command is ON. <Program>… -
Page 28: Program/Sequence/Block Numbers ; L(O), N
3. Data Formats 3.5 Program/Sequence/Block Numbers ; L(O), N 3.5 Program/Sequence/Block Numbers ; L(O), N Function and purpose These numbers are used for monitoring the execution of the machining programs and for calling both machining programs and specific stages in machining programs. (1) Program numbers are classified by workpiece correspondence or by subprogram units, and they are designated by the address «L»…
-
Page 29: Parity H/V
3. Data Formats 3.6 Parity H/V 3.6 Parity H/V Function and purpose Parity check provides a mean of checking whether the tape has been correctly perforated or not. This involves checking for perforated code errors or, in other words, for perforation errors. There are two types of parity check: Parity H and Parity V.
-
Page 30: G Code Lists
3. Data Formats 3.7 G Code Lists 3.7 G Code Lists Function and purpose G code Group Function Section Δ 00 Positioning Δ 01 Linear interpolation Circular interpolation CW (clockwise) R-specified circular interpolation CW Helical interpolation CW Spiral/Conical interpolation CW (type2) 6.13 Circular interpolation CCW (counterclockwise) R-specified circular interpolation CCW…
-
Page 31
3. Data Formats 3.7 G Code Lists G code Group Function Section Subprogram call / figure rotation ON 13.3 Subprogram return / figure rotation cancel 13.3 22.1 Stroke check before travel ON 15.7 23.1 Stroke check before travel cancel 15.7 Reference position check 14.9 Reference position return… -
Page 32
3. Data Formats 3.7 G Code Lists G code Group Function Section * 50 Scaling cancel 13.20 Scaling ON 13.20 * 50.1 G command mirror image cancel 13.6 51.1 G command mirror image ON 13.6 Local coordinate system setting 14.11 Basic machine coordinate system selection 14.4 * 54… -
Page 33: Precautions Before Starting Machining
3. Data Formats 3.8 Precautions Before Starting Machining G code Group Function Section Δ 90 Absolute value command Δ 91 Incremental command value Coordinate system setting / Spindle clamp speed setting 14.5 92.1 Workpiece coordinate system pre-setting 14.12 Inverse time feed Δ…
-
Page 34: Buffer Register
4. Buffer Register 4.1 Input Buffer 4. Buffer Register 4.1 Input Buffer Function and purpose When the pre-read buffer is empty during a tape operation or RS232C operation, the contents of the input buffer are immediately transferred to the pre-read buffers and, provided that the data stored in the input buffer do not exceed 250 x 4 characters, the following data (Max.
-
Page 35: Pre-Read Buffers
4. Buffer Register 4.2 Pre-read Buffers 4.2 Pre-read Buffers Function and purpose During automatic processing, the contents of 1 block are normally pre-read so that program analysis processing is conducted smoothly. However, during tool radius compensation, a maximum of 5 blocks are pre-read for the intersection point calculation including interference check.
-
Page 36: Position Commands
5. Position Commands 5.1 Position Command Methods ; G90, G91 5. Position Commands 5.1 Position Command Methods ; G90, G91 Function and purpose By using the G90 and G91 commands, it is possible to execute the next coordinate commands using absolute values or incremental values. The R-designated circle radius and the center of the circle determined by I, J, K are always incremental value commands.
-
Page 37
5. Position Commands 5.1 Position Command Methods ; G90, G91 (3) Since multiple commands can be issued in the same block, it is possible to command specific addresses as either absolute values or incremental 200. values. N 4 G90 X300. G91 Y100.; 100. -
Page 38: Inch/Metric Command Change; G20, G21
5. Position Commands 5.2 Inch/Metric Command Change; G20, G21 5.2 Inch/Metric Command Change; G20, G21 Function and purpose These G commands are used to change between the inch and millimeter (metric) systems. Command format G20/G21; : Inch command : Metric command Detailed description The G20 and G21 commands merely select the command units.
-
Page 39
5. Position Commands 5.2 Inch/Metric Command Change; G20, G21 Precautions (1) The parameter and tool data will be input/output with the «#1041 I_inch» setting unit. If «#1041 I_inch» is not found in the parameter input data, the unit will follow the unit currently set to NC. -
Page 40: Decimal Point Input
5. Position Commands 5.3 Decimal Point Input 5.3 Decimal Point Input Function and purpose This function enables the decimal point command to be input. It assigns the decimal point in millimeter or inch units for the machining program input information that defines the tool paths, distances and speeds.
-
Page 41
5. Position Commands 5.3 Decimal Point Input Example of program Example of program for decimal point valid address Specification Decimal point Decimal point command 1 division command 2 When 1 = 1μm When 1 = 10μm 1 = 1mm Program example G0X123.45 (decimal points are all mm X123.450mm… -
Page 42
5. Position Commands 5.3 Decimal Point Input Addresses used and validity/invalidity of decimal point commands are shown below. Decimal point Address Application Remarks command Valid Coordinate position data Invalid Revolving table Invalid Miscellaneous function code Valid Angle data Invalid Data settings, axis numbers (G10) Invalid Subprogram call : program No. -
Page 43
5. Position Commands 5.3 Decimal Point Input Decimal point Address Application Remarks command Valid Arc center coordinates Invalid Center of figure rotation (incremental) Valid Tool radius compensation vector components Valid Special fixed cycle’s hole pitch or angle Valid G0/G1 imposition width, drilling cycle G1 imposition width Valid Stroke check before travel: lower limit coordinates Valid… -
Page 44
5. Position Commands 5.3 Decimal Point Input Decimal point Address Application Remarks command Valid Cut amount of deep hole drill cycle Valid Shift amount of back boring Valid Shift amount of fine boring Invalid Minimum spindle clamp speed Valid Starting shift angle for screw cutting Invalid Transmission destination variable No. -
Page 45: Interpolation Functions
6. Interpolation Functions 6.1 Positioning (Rapid Traverse) 6. Interpolation Functions 6.1 Positioning (Rapid Traverse); G00 Function and purpose This command is accompanied by coordinate words. It positions the tool along a linear or non-linear path from the present point as the start point to the end point which is specified by the coordinate words.
-
Page 46
6. Interpolation Functions 6.1 Positioning (Rapid Traverse) Example of program +300 Tool End point (-120,+200,+300) +150 Start point -100 (+150,-100,+150) -120 Unit : mm +150 +200 G91 G00 X-270000 Y300000 Z150000 ; (For input setting unit: 0.001mm) (Note 1) When parameter «#1086 G0Intp» is set to «0», the path along which the tool is positioned is the shortest path connecting the start and end points. -
Page 47
6. Interpolation Functions 6.1 Positioning (Rapid Traverse) (Note 2) When parameter «#1086 G0Intp» is set to 1, the tool will move along the path from the start point to the end point at the rapid traverse rate of each axis. When, for instance, the Y axis and Z axis rapid traverse rates are both 9600mm/min, the tool will follow the path in the figure below if the following is programmed: G91 G00 X-300000 Y200000 ;… -
Page 48
6. Interpolation Functions 6.1 Positioning (Rapid Traverse) (Note 4) Rapid traverse (G00) deceleration check There are two methods for the deceleration check at rapid traverse; commanded deceleration method and in-position check method. Select a method with the parameter «#1193 inpos». ■… -
Page 49
6. Interpolation Functions 6.1 Positioning (Rapid Traverse) (3) Exponential acceleration/exponential deceleration ….. Td = 2 × Ts + α Previous block Next block Ts : Acceleration/deceleration time constant Td : Deceleration check time Td = 2 × Ts + (0 ~ 14ms) Where Ts is the acceleration time constant, α… -
Page 50
6. Interpolation Functions 6.1 Positioning (Rapid Traverse) Programmable in-position width command for positioning This command commands the in-position width for the positioning command from the machining program. G00 X__ Y__ Z__ , I__ ; In-position width Positioning coordinate value of each axis Operation during in-position check Execution of the next block starts after confirming that the position error amount of the positioning (rapid traverse: G00) command block and the block that carries out deceleration check with the… -
Page 51
6. Interpolation Functions 6.1 Positioning (Rapid Traverse) In-position width setting When the servo parameter «#2224 SV024» setting value is smaller than the setting value of the G0 in-position width «#2077 G0inps» and the G1 in-position width «#2078 G1inps», the in-position check is carried out with the G0 in-position width and the G1 in-position width. -
Page 52: Linear Interpolation; G01
6. Interpolation Functions 6.2 Linear Interpolation 6.2 Linear Interpolation; G01 Function and purpose This command is accompanied by coordinate words and a feedrate command. It makes the tool move (interpolate) linearly from its present position to the end point specified by the coordinate words at the speed specified by address F.
-
Page 53
6. Interpolation Functions 6.2 Linear Interpolation Example of program → P → P → P → P (Example 1) Cutting in the sequence of P at 300 mm/min feedrate → P is for tool positioning Unit: mm Input setting unit: 0.001mm →… -
Page 54: Plane Selection; G17, G18, G19
6. Interpolation Functions 6.3 Plane Selection 6.3 Plane Selection; G17, G18, G19 Function and purpose The plane to which the movement of the tool during the circle interpolation (including helical cutting) and tool radius compensation command belongs is selected. By registering the basic three axes and the corresponding parallel axis as parameters, a plane can be selected by two axes that are not the parallel axis.
-
Page 55
6. Interpolation Functions 6.3 Plane Selection Plane selection system In Table 1, I is the horizontal axis for the G17 plane or the vertical axis for the G18 plane J is the vertical axis for the G17 plane or the horizontal axis for the G19 plane K is the horizontal axis for the G18 plane or the vertical axis for the G19 plane In other words, G17 .. -
Page 56: Circular Interpolation; G02, G03
6. Interpolation Functions 6.4 Circular Interpolation 6.4 Circular Interpolation; G02, G03 Function and purpose These commands serve to move the tool along an arc. Command format G02 (G03) X__ Y__ I__ J__ K__ F__; : Clockwise (CW) : Counterclockwise (CCW) X, Y : End point I, J…
-
Page 57
6. Interpolation Functions 6.4 Circular Interpolation Detailed description (1) G02 (or G03) is retained until another G command (G00, G01 or G33) in the 01 group that changes its mode is issued. The arc rotation direction is distinguished by G02 and G03. G02 Clockwise (CW) G03 Counterclockwise (CCW) G17(X-Y)plane… -
Page 58
6. Interpolation Functions 6.4 Circular Interpolation Example of program (Example 1) Y axis Feedrate Circle center F = 500mm/min J = 50mm X axis Start point/end point G02 J50000 F500 ; Circle command (Example 2) Y axis Feedrate End point Arc center F = 500mm/min X50 Y50mm… -
Page 59
6. Interpolation Functions 6.4 Circular Interpolation Plane selection The planes in which the arc exists are the following three planes (refer to the detailed drawings), and are selected with the following method. XY plane G17; Command with a (plane selection G code) ZX plane G18;… -
Page 60
6. Interpolation Functions 6.4 Circular Interpolation Precautions for circular interpolation (1) The terms «clockwise» (G02) and «counterclockwise» (G03) used for arc operations are defined as a case where in a right-hand coordinate system, the negative direction is viewed from the position direction of the coordinate axis which is at right angles to the plane in question. -
Page 61: R-Specified Circular Interpolation; G02, G03
6. Interpolation Functions 6.5 R-specified Circular Interpolation 6.5 R-specified Circular Interpolation; G02, G03 Function and purpose Along with the conventional circular interpolation commands based on the arc center coordinate (I, J, K) designation, these commands can also be issued by directly designating the arc radius R. Command format G02 (G03) X__ Y__ R__ F__ ;…
-
Page 62
6. Interpolation Functions 6.5 R-specified Circular Interpolation Example of program (Example 1) G02 Xx XY plane R-specified arc (Example 2) G03 Zz ZX plane R-specified arc (Example 3) G02 Xx XY plane R-specified arc (When the R specification and I, J, (K) specification are contained in the same block, the R specification has priority in processing.) (Example 4) -
Page 63
6. Interpolation Functions 6.5 R-specified Circular Interpolation Circular center coordinate compensation When «the error margin between the segment connecting the start and end points» and «the commanded radius × 2» is less than the setting value because the required semicircle is not obtained by calculation error in R specification circular interpolation, «the midpoint of segment connecting the start and end points»… -
Page 64: Helical Interpolation ; G17 To G19, G02, G03
6. Interpolation Functions 6.6 Helical Interpolation 6.6 Helical Interpolation ; G17 to G19, G02, G03 Function and purpose While circular interpolating with G02/G03 within the plane selected with the plane selection G code (G17, G18, G19), the 3rd axis can be linearly interpolated. Normally, the helical interpolation speed is designated with the tangent speed F’ including the 3rd axis interpolation element as shown in the lower drawing of Fig.
-
Page 65
6. Interpolation Functions 6.6 Helical Interpolation The arc plane element speed designation and normal speed designation can be selected with the parameter. #1235 set07/bit0 Meaning Arc plane element speed designation is selected. Normal speed designation is selected. Normal speed designation θ… -
Page 66
6. Interpolation Functions 6.6 Helical Interpolation The plane for an additional axis can be selected as with circular interpolation. UY plane circular, Z axis linear Command the U, Y and Z axis addresses in the G02 (G03) and G19 (plane selection G code) mode. -
Page 67
6. Interpolation Functions 6.6 Helical Interpolation (Example 4) U axis X axis Z axis G18 G03 Xx Ii1 Kk ZX plane arc, U axis linear (Note) If the same system is used, the standard axis will perform circular interpolation and the additional axis will perform linear interpolation. (Example 5) G18 G02 Xx ZX plane arc, U axis, Y axis linear… -
Page 68: Thread Cutting
6. Interpolation Functions 6.7 Thread Cutting 6.7 Thread Cutting 6.7.1 Constant Lead Thread Cutting; G33 Function and purpose The G33 command exercises feed control over the tool which is synchronized with the spindle rotation and so this makes it possible to conduct constant-lead straight thread-cutting and tapered thread-cutting.
-
Page 69
6. Interpolation Functions 6.7 Thread Cutting Thread cutting metric input Input unit B (0.001mm) C (0.0001mm) system Command F (mm/rev) E (mm/rev) E (ridges/inch) F (mm/rev) E (mm/rev) E (ridges/inch) address Minimum 1(=1.000) 1(=1.00000) 1(=1.00) 1(=1.0000) 1(=1.000000) 1(=1.000) command (1.=1.000) (1.=1.00000) (1.=1.00) (1.=1.0000) -
Page 70
6. Interpolation Functions 6.7 Thread Cutting (6) If the feed hold function is employed during thread cutting to stop the feed, the thread ridges will lose their shape. For this reason, feed hold does not function during thread cutting. Note that this is valid from the time the thread cutting command is executed to the time the axis moves. -
Page 71
6. Interpolation Functions 6.7 Thread Cutting Example of program N110 G90 G0 X-200. Y-200. S50 M3 ; The spindle center is positioned to the workpiece center, and the spindle rotates in the forward direction. N111 Z110. ; N112 G33 Z40. F6.0 ; The first thread cutting is executed. -
Page 72: Inch Thread Cutting; G33
6. Interpolation Functions 6.7 Thread Cutting 6.7.2 Inch Thread Cutting; G33 Function and purpose If the number of ridges per inch in the long axis direction is assigned in the G33 command, the feed of the tool synchronized with the spindle rotation will be controlled, which means that constant-lead straight thread-cutting and tapered thread-cutting can be performed.
-
Page 73: Unidirectional Positioning; G60
6. Interpolation Functions 6.8 Unidirectional Positioning Example of program Thread lead ..3 threads/inch (= 8.46666 …) When programmed with δ = 10mm, δ = 10mm using metric input δ 50.0mm δ N210 G90 G0X-200. Y-200. S50M3; N211 Z110.; N212 G91 G33 Z-70.E3.0; (First thread cutting) N213 M19;…
-
Page 74
6. Interpolation Functions 6.8 Unidirectional Positioning Command format G60 X__ Y__ Z__ α__ ; α : Optional axis Detailed description (1) The creep distance for the final positioning as well as the final positioning direction is set by parameter. (2) After the tool has moved at the rapid traverse rate to the position separated from the final position by an amount equivalent to the creep distance, it move to the final position in accordance with the rapid traverse setting where its positioning is completed. -
Page 75: Cylindrical Interpolation; G07.1
6. Interpolation Functions 6.9 Cylindrical Interpolation ; G07.1 6.9 Cylindrical Interpolation; G07.1 Function and purpose This function develops a shape with a cylindrical side (shape in cylindrical coordinate system) into a plane. When the developed shape is programmed as the plane coordinates, that is converted into the linear axis and rotation axis movement in the cylindrical coordinates and the contour is controlled during machining.
-
Page 76
6. Interpolation Functions 6.9 Cylindrical Interpolation ; G07.1 Command format G07.1 C__ ; (Cylindrical interpolation mode start/cancel) : Cylinder radius value • Radius value ≠ 0: Cylindrical interpolation mode start • Radius value = 0: Cylindrical interpolation mode cancel (Note) The above format applies when the name of the rotation axis is «C». If the name is not «C», command the name of the rotation axis being used instead of «C». -
Page 77
6. Interpolation Functions 6.9 Cylindrical Interpolation ; G07.1 Detailed description (1) Command G07.1 in an independent block. A program error (P33) will occur if this command is issued in the same block as another G code. (2) Program the rotation axis with an angle degree. (3) Linear interpolation or circular interpolation can be commanded during the cylindrical interpolation mode. -
Page 78
6. Interpolation Functions 6.9 Cylindrical Interpolation ; G07.1 (9) Plane selection (Note) The axis used for cylindrical interpolation must be set with the plane selection command. The correspondence of the rotation axis to an axis’ parallel axis is set with the parameters (#1029, #1030, #1031). -
Page 79
6. Interpolation Functions 6.9 Cylindrical Interpolation ; G07.1 (10) Related parameters Setting Item Details range 1516 mill_ax Milling axis Set the name of the rotation axis for milling interpolation A to Z name (pole coordinate interpolation, cylindrical interpolation). Only one of the rotation axes can be set. 8111 Milling Radius Select the diameter and radius of the linear axis for milling… -
Page 80
6. Interpolation Functions 6.9 Cylindrical Interpolation ; G07.1 (3) Tool radius compensation The tool radius can be compensated during the cylindrical interpolation mode. (a) Command the plane selection in the same manner as circular interpolation. When using tool radius compensation, start up and cancel the compensation within the cylindrical interpolation mode. -
Page 81
6. Interpolation Functions 6.9 Cylindrical Interpolation ; G07.1 Restrictions and precautions (1) The cylindrical interpolation mode is canceled when the power is turned ON or reset. (2) A program error (P484) will occur if any axis commanded for cylindrical interpolation has not completed reference position return. -
Page 82
6. Interpolation Functions 6.9 Cylindrical Interpolation ; G07.1 Example of program <Program> <Parameter> N01 G28XZC; #1029 aux_I N02 G97S100M23; #1030 aux_J N03 G00X50.Z0.; #1031 aux_K N04 G94G01X40.F100.; Command of plane selection for cylindrical interpolation N05 G19C0Z0; and command of two interpolation axes N06 G07.1C20.;… -
Page 83: Polar Coordinate Interpolation; G12.1, G13.1
6. Interpolation Functions 6.10 Polar Coordinate Interpolation; G12.1, G13.1 6.10 Polar Coordinate Interpolation; G12.1, G13.1 Function and purpose This function converts the commands programmed with the orthogonal coordinate axis into linear axis movement (tool movement) and rotation axis movement (workpiece rotation), and controls the contour.
-
Page 84
6. Interpolation Functions 6.10 Polar Coordinate Interpolation; G12.1, G13.1 Detailed description (1) Command G12.1 and G13.1 in an independent block. A program error (P33) will occur if this command is issued in the same block as another G code. (2) Linear interpolation or circular interpolation can be commanded during the pole coordinate interpolation mode. -
Page 85
6. Interpolation Functions 6.10 Polar Coordinate Interpolation; G12.1, G13.1 (8) F command during pole coordinate interpolation As for the F command in the pole coordinate interpolation mode, whether the previous F command is used or not depends on that the mode just before G12.1 is the feed per minute command (G94/G98) or feed per rotation command (G95/G99). -
Page 86
6. Interpolation Functions 6.10 Polar Coordinate Interpolation; G12.1, G13.1 Relation with other functions (1) The following G code commands can be used during the pole coordinate interpolation mode. G code Details Positioning Linear interpolation Circular interpolation (CW) Circular interpolation (CWW) Dwell Exact stop check G40-42… -
Page 87
6. Interpolation Functions 6.10 Polar Coordinate Interpolation; G12.1, G13.1 (4) Tool radius compensation The tool radius can be compensated during the pole coordinate interpolation mode. (a) Command the plane selection in the same manner as pole coordinate interpolation. When using tool radius compensation, it must be started up and canceled within the pole coordinate interpolation mode. -
Page 88
6. Interpolation Functions 6.10 Polar Coordinate Interpolation; G12.1, G13.1 (8) Hole drilling axis in the hole drilling fixed cycle command during the pole coordinate interpolation Hole drilling axis in the hole drilling fixed cycle command during the pole coordinate interpolation is determined with the linear axis parameter (#1533). #1533 setting value Hole drilling axis Z (pole coordinate plane is interpreted as XY plane) -
Page 89
6. Interpolation Functions 6.10 Polar Coordinate Interpolation; G12.1, G13.1 (11) A program error (P486) will occur if the cylindrical interpolation or the pole coordinate interpolation is commanded during the pole coordinate interpolation mode. (12) During pole coordinate interpolation, if X axis moveable range is controlled in the plus side, X axis has to be moved to the plus area that includes «0»… -
Page 90: Exponential Function Interpolation; G02.3, G03.3
6. Interpolation Functions 6.11 Exponential Function Interpolation; G02.3, G03.3 6.11 Exponential Function Interpolation; G02.3, G03.3 Function and purpose Exponential function interpolation changes the rotation axis into an exponential function shape in respect to the linear axis movement. At this time, the other axes carry out linear interpolation between the linear axis. This allows a machining of a taper groove with constant torsion angle (helix angle) (uniform helix machining of taper shape).
-
Page 91
6. Interpolation Functions 6.11 Exponential Function Interpolation; G02.3, G03.3 Command format G02.3/G03.3 Xx1 Yy1 Zz1 Ii1 Jj1 Rr1 Ff1 Qq1 Kk1 ; G02.3 : Forward rotation interpolation (modal) G03.3 : Negative rotation interpolation (modal) : X axis end point (Note 1) : Y axis end point (Note 1) : Z axis end point (Note 1) : Angle i1 (Note 2) -
Page 92
6. Interpolation Functions 6.11 Exponential Function Interpolation; G02.3, G03.3 (Note 5) The command unit is as follows. Setting unit #1003 = B #1003 = C #1003 = D #1003 = E Unit Metric system 0.001 0.0001 0.00001 0.000001 Inch system 0.0001 0.00001 0.000001… -
Page 93
6. Interpolation Functions 6.11 Exponential Function Interpolation; G02.3, G03.3 Machining example • Example of uniform helix machining of taper shape Z axis A axis X axis <Relational expression of exponential function in machining example> θ /D Z (θ) = r1 ∗ (e -1) ∗… -
Page 94
6. Interpolation Functions 6.11 Exponential Function Interpolation; G02.3, G03.3 The taper gradient angle (i1) and torsion angle (j1) are each issued with the command address I and J. Note that if the shape is a reverse taper shape, the taper gradient angle (i1) is issued as a negative value. -
Page 95
6. Interpolation Functions 6.11 Exponential Function Interpolation; G02.3, G03.3 Precautions for programming (1) When G02.3/G03.3 is commanded, interpolation takes place with the exponential function relational expression using the start position of the linear axis and rotation axis as 0. (2) Linear interpolation will take place in the following cases, even if in the G02.3/G03.3 mode. The feedrate for linear interpolation will be the F command in that block. -
Page 96: Polar Coordinate Command; G16/G15
6. Interpolation Functions 6.12 Polar Coordinate Command; G16/G15 6.12 Polar Coordinate Command; G16/G15 Function and purpose With this function, the end point coordinate value is commanded with the polar coordinate of the radius and angle. Command format G16 ; Polar coordinate command mode ON G15 ;…
-
Page 97
6. Interpolation Functions 6.12 Polar Coordinate Command; G16/G15 (7) When the radius is commanded with the absolute value, command the distance from the zero point in the workpiece coordinate system (note that the local coordinate system is applied when the local coordinate system is set). (8) When the radius is commanded with the incremental value command, considering the end point of the previous block as the polar coordinate center, command the incremental value from that end point. -
Page 98
6. Interpolation Functions 6.12 Polar Coordinate Command; G16/G15 (3) When the radius command is omitted When the radius command is omitted, the zero point in the workpiece coordinate system is applied to the polar coordinate center, and the distance between the polar coordinate center and current position is regarded as the radius. -
Page 99
6. Interpolation Functions 6.12 Polar Coordinate Command; G16/G15 Axis command not interpreted as polar coordinate command The axis command with the following command is not interpreted as the polar coordinate command during the polar coordinate command mode. The movement command that has no axes commands for the 1st axis and 2nd axis in the selected plane mode is also not interpreted as polar coordinate command during the polar coordinate command mode. -
Page 100
6. Interpolation Functions 6.12 Polar Coordinate Command; G16/G15 Example of program When the zero point in the workpiece coordinate system is the polar coordinate zero point • The polar coordinate zero point is the zero point in the workpiece coordinate system. -
Page 101
6. Interpolation Functions 6.12 Polar Coordinate Command; G16/G15 Precautions (1) If the following commands are carried out during the polar coordinate command mode, or if the polar coordinate command is carried out during the following command mode, a program error (P34) will occur. -
Page 102: Spiral/Conical Interpolation; G02.0/G03.1(Type1), G02/G03(Type2)
6. Interpolation Functions 6.13 Spiral/Conical Interpolation 6.13 Spiral/Conical Interpolation; G02.0/G03.1(Type1), G02/G03(Type2) Function and purpose This function carries out interpolation that smoothly joins the start and end points in a spiral. This interpolation is carried out for arc commands in which the start point and end point are not on the same circumference.
-
Page 103
6. Interpolation Functions 6.13 Spiral/Conical Interpolation (5) P designates the number of pitches (number of spirals). (Type 1) The number of pitches and rotations is as shown below. Number of pitches Number of rotations (0 to 99) Less than 1 rotation (Can be omitted.) 1 or more rotation, less than 2 rotations… -
Page 104
6. Interpolation Functions 6.13 Spiral/Conical Interpolation (9) In the following cases, a program error will occur. (a) Items common for type 1 and 2 Command Settings Error range (Unit) End point Range of • If a value exceeding the command range is issued, coordinate coordinate program error (P35) will occur. -
Page 105
6. Interpolation Functions 6.13 Spiral/Conical Interpolation Detailed description (1) The arc rotation direction G02.1 is the same as G02, and G03.1 is the same as G03. (2) There are no R-designated arcs in spiral interpolation. (3) Conical cutting, tapered thread-cutting and other such machining operations can be conducted by changing the start point and end point radius and commanding the linear axis simultaneously. -
Page 106
6. Interpolation Functions 6.13 Spiral/Conical Interpolation Example of program (Example 1) G91 G17 G01 X60. F500 ; Y140. ; G02.1 X60. Y0 I100. P1 F300 ; point G01 X−120 ; Center 140. Start point G17 G01 X60. F500 ; Y140. ; X60. -
Page 107: 3-Dimensional Circular Interpolation; G02.4, G03.4
6. Interpolation Functions 6.14 3-dimensional Circular Interpolation; G02.4, G03.4 6.14 3-dimensional Circular Interpolation; G02.4, G03.4 Function and purpose To issue a circular command over a 3-dimensional space, an arbitrary point (intermediate point) must be designated on the arc in addition to the start point (current position) and end point. By using the 3-dimensional circular interpolation command, an arc shape determined by the three points (start point, intermediate point, end point) designated on the 3-dimensional space can be machined.
-
Page 108
6. Interpolation Functions 6.14 3-dimensional Circular Interpolation; G02.4, G03.4 Command format α α1 G02.4(G03.4) Xx1 Yy1 Zz1 ; Intermediate point designation (1st block) α α2 Xx2 Yy2 Zz2 ; End point designation (2nd block) G02.4(G03.4) : 3-dimensional circular interpolation command (Cannot designate the rotation direction) x1, y1, z1 : Intermediate point coordinates x2, y2, z2… -
Page 109
6. Interpolation Functions 6.14 3-dimensional Circular Interpolation; G02.4, G03.4 Designating intermediate point and end point When using the 3-dimensional circular interpolation command, an arc that exists over the 3-dimensional space can be determined by designating the intermediate point and end point in addition to the start point (current position). -
Page 110
6. Interpolation Functions 6.14 3-dimensional Circular Interpolation; G02.4, G03.4 When liner interpolation is applied In the following case, liner interpolation but 3-dimensional circular interpolation is applied. (1) When the start point, intermediate point, and end point are on the same line (refer to the following figure) (If the end point exists between the start point and intermediate point, axes move in the order of start point, intermediate point, and end point.) -
Page 111
6. Interpolation Functions 6.14 3-dimensional Circular Interpolation; G02.4, G03.4 Relation with other functions (1) Commands that cannot be used (a) G code command which leads to a program error during 3-dimensional circular interpolation modal G code Function name Program error G05 Pn High-speed machining mode G05 P10000… -
Page 112: Nurbs Interpolation
6. Interpolation Functions 6.15 NURBS Interpolation 6.15 NURBS Interpolation Function and purpose This function realizes NURBS (Non-Uniform Rational B-Spline) curve machining by simply commanding NURBS curve parameters (stage, weight, knot, control point), which is used for the curved surface/line machining, without replacing the path with minute line segments. This function operates only in the high-speed high-accuracy control II mode, so the high-speed high-accuracy control II option is required.
-
Page 113
6. Interpolation Functions 6.15 NURBS Interpolation Detailed description (1) Designate the stage P for the 1st block of NURBS interpolation. (2) Designate the same coordinate value for the 1st block control point of NURBS interpolation as that designated right before NURBS interpolation. (3) Designate all axes to be used in the subsequent NURBS interpolation blocks for 1st block of NURBS interpolation (4) Set the same value for knot K from the 1st block of NURBS interpolation to setting value block… -
Page 114
6. Interpolation Functions 6.15 NURBS Interpolation Example of program The example of program that has 4 stages (cubic curve) and 11 control points is shown below. Control point Knot G05 P10000; P10(9.5,8.0) G90 G01 X0. Y0. Z0. F300; G06.2 P4 X0. Y0. R1. K0; P9(8.0,6.5) X1.0 Y2.0 R1. -
Page 115
6. Interpolation Functions 6.15 NURBS Interpolation Relation with other functions (1) G code/Feed/Miscellaneous functions All the G code, feedrate and MSTB code cannot be set during NURBS interpolation. However, when the fixed cycle G code is commanded in the same block where G06.2 is commanded, the fixed cycle G code is ignored. -
Page 116
6. Interpolation Functions 6.15 NURBS Interpolation Precautions (1) Target axes for NURBS interpolation are 3 basic axes. (2) Command the control point for all the axes for which NURBS interpolation is carried out in the 1st block (G06.2 block). A program error (P32) will occur if an axis which was not commanded in the 1st block is commanded in the 2nd block or after. -
Page 117: Hypothetical Axis Interpolation; G07
6. Interpolation Functions 6.16 Hypothetical Axis Interpolation; G07 6.16 Hypothetical Axis Interpolation; G07 Function and purpose Take one of the axes of the helical interpolation or spiral interpolation, including a linear axis, as a hypothetical axis (axis with no actual movement) and perform pulse distribution. With this procedure, an interpolation equivalent to the helical interpolation or spiral interpolation looked from the side (hypothetical axis), or SIN or COS interpolation, will be possible.
-
Page 118
6. Interpolation Functions 6.16 Hypothetical Axis Interpolation; G07 Detailed description α α α (1) During “G07 0” to “G07 1”, axis will be the hypothetical axis. (2) Any axis among the NC axes can be designated as the hypothetical axis. (3) Multiple axes can be designated as the hypothetical axis. -
Page 119: Feed Functions
7. Feed Functions 7.1 Rapid Traverse Rate 7. Feed Functions 7.1 Rapid Traverse Rate Function and purpose The rapid traverse rate can be set independently with parameters for each axis. The available speed ranges are from 1 mm/min to 10000000 mm/min. The upper limit is subject to the restrictions imposed by the machine specifications.
-
Page 120: F1-Digit Feed
7. Feed Functions 7.3 F1-digit Feed 7.3 F1-digit Feed Function and purpose By setting the F1-digit feed parameter, the feedrate which has been set to correspond to the 1-digit number following the F address serves as the command value. When F0 is assigned, the rapid traverse rate is established and the speed is the same as for G00. (G modal does not change, but the acceleration/deceleration method is followed by the settings for the rapid…
-
Page 121
7. Feed Functions 7.3 F1-digit Feed When F1. to F5. (with decimal point) are assigned, the 1mm/min to 5mm/min direct commands are established instead of the F1-digit command. When the commands are used with the millimeter or degree units, the feedrate set to correspond to F1 to F5 serves as the assigned speed mm (°)/min. -
Page 122: Per-Minute/Per-Revolution Feed (Asynchronous/Synchronous Feed); G94, G95
7. Feed Functions 7.4 Per-minute/Per-revolution Feed (Asynchronous/Synchronous Feed); G94, G95 7.4 Per-minute/Per-revolution Feed (Asynchronous/Synchronous Feed); G94, G95 Function and purpose Using the G95 command, it is possible to assign the feed amount per rotation with an F code. When this command is used, the rotary encoder must be attached to the spindle. When the G94 command is issued the per-minute feed rate will return to the designated per-minute feed (asynchronous feed) mode.
-
Page 123
7. Feed Functions 7.4 Per-minute/Per-revolution Feed (Asynchronous/Synchronous Feed); G94, G95 Inch input Input B (0.0001inch) C (0.00001inch) command unit system Command Feed per minute Feed per rotation Feed per minute Feed per rotation mode Command F (inch/min) E (inch/rev) F (inch/min) E (inch/rev) address Minimum… -
Page 124: Inverse Time Feed; G93
7. Feed Functions 7.5 Inverse Time Feed; G93 7.5 Inverse Time Feed; G93 Function and purpose During inside cutting when machining curved shapes with radius compensation applied, the machining speed on the cutting surface becomes faster than the tool center feedrate. Therefore, problems such as reduced accuracy may occur.
-
Page 125
7. Feed Functions 7.5 Inverse Time Feed; G93 Detailed description (1) Inverse time feed (G93) is a modal command. Once commanded, it is valid until feed per minute (G94) or feed per revolution (G95) is commanded, or until a reset (M02, M30, etc.) is executed. -
Page 126
7. Feed Functions 7.5 Inverse Time Feed; G93 Example of program When using inverse time feed during tool radius compensation Feed per minute N01 G90 G00 X80. Y-80. ; N02 G01 G41 X80 Y-80. D11 F500 ; N03 X180. ; N04 G02 Y-280. -
Page 127
7. Feed Functions 7.5 Inverse Time Feed; G93 Relation with other functions (1) Scaling (G51) When using a scaling function, issue a F command for the shape after scaling. For example, if a double-size scaling is carried out, the machining distance will be twice. Thus, if executing a cutting at the same speed as that of before scaling, command the value (F’) calculated by dividing F value by the multiples of scaling. -
Page 128: Feedrate Designation And Effects On Control Axes
7. Feed Functions 7.6 Feedrate Dsignation and Effects on Control Axes 7.6 Feedrate Designation and Effects on Control Axes Function and purpose It has already been mentioned that a machine has a number of control axes. These control axes can be divided into linear axes which control linear movement and rotary axes which control rotary movement.
-
Page 129
7. Feed Functions 7.6 Feedrate Dsignation and Effects on Control Axes (Example) When the feedrate is designated as «f» and the linear axes (X and Y) are to be controlled using the circular interpolation function: The rate in the tool advance direction, or in other words the tangential direction, will be the feedrate designated in the program. -
Page 130
7. Feed Functions 7.6 Feedrate Dsignation and Effects on Control Axes When linear and rotary axes are to be controlled at the same time The controller proceeds in exactly the same way whether linear or rotary axes are to be controlled. When a rotary axis is to be controlled, the numerical value assigned by the coordinate word (A, B, C) is the angle and the numerical values assigned by the feedrate (F) are all handled as linear speeds. -
Page 131
7. Feed Functions 7.6 Feedrate Dsignation and Effects on Control Axes X-axis feedrate (linear speed) «fx» and C-axis feedrate (angular speed) «ω» are expressed as: fx = f × ………………(1) ω = f × ………………(2) Linear speed «fc» based on C-axis control is expressed as: π… -
Page 132: Rapid Traverse Constant Inclination Acceleration/Deceleration
7. Feed Functions 7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration 7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration Function and purpose This function performs acceleration and deceleration at a constant inclination during linear acceleration/deceleration in the rapid traverse mode. Compared to the method of acceleration /deceleration after interpolation, the constant inclination acceleration/deceleration method makes for improved cycle time.
-
Page 133
7. Feed Functions 7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration (3) When 2-axis simultaneous interpolation (linear interpolations) is performed during rapid traverse constant inclination acceleration and deceleration, the acceleration (deceleration) time is the longest value of the acceleration (deceleration) times determined for each axis by the rapid traverse rate of commands executed simultaneously, the rapid traverse acceleration and deceleration time constant, and the interpolation distance, respectively. -
Page 134: Rapid Traverse Constant Inclination Multi-Step Acceleration/Deceleration
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration Function and purpose This function carries out the acceleration/deceleration according to the torque characteristic of the motor in the rapid traverse mode during automatic operation. (This function is not available in manual operation.) The rapid traverse constant inclination multi-step acceleration/deceleration method makes for improved cycle time because the positioning time is shortened by using the motor ability to its maximum.
-
Page 135
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration Speed Speed Time Time Acceler- Acceler- Number of steps is ation ation automatically adjusted It was necessary to slow down the by parameter setting. acceleration for high speed rotation. Time Time (a) Rapid traverse constant inclination multi-step (b) Rapid traverse constant inclination… -
Page 136
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration Speed Rapid traverse rate Rated speed Time Acceleration time to rated speed Acceleration Max. acceleration Acceleration at rapid traverse rate Time Acceleration at rapid traverse rate Acceleration rate in proportion to the maximum acceleration rate Max. -
Page 137
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration (4) The comparison of the acceleration/deceleration patterns by the parameter setting is in the table below. Rapid traverse constant #1086 #1205 Mode Operation inclination multi-step G00Intp G0bdcc acceleration/deceleration Time constant command acceleration/deceleration (interpolation type) -
Page 138
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration Detailed description (decision method of steps) For rapid traverse constant inclination multi-step acceleration/deceleration, the number of steps is automatically adjusted by set parameter. The acceleration per step is assumed to be a decrease by 10% of the maximum acceleration per step. -
Page 139
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration Detailed description (Acceleration pattern at two or more axis interpolation) When there are two or more rapid traverse axes with a different acceleration pattern, there are the following two operation methods. •… -
Page 140
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration Detailed description (S-pattern filter control) With S-pattern filter control, this enables the rapid traverse inclination multi-step acceleration/ deceleration fluctuation to further smoothen. This can be set in the range of 0 to 200 (ms) with the basic specification parameter «#1569 SfiltG0» (G00 soft acceleration/deceleration filter). -
Page 141
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration Speed Larger than the rated speed Rapid traverse date The high-accuracy control mode rapid traverse rate Rated speed Time Acceleration time to rated speed Acceleration Max. Acceleration Acceleration at rapid traverse rate Time Smaller than the rated speed… -
Page 142
7. Feed Functions 7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration Rapid traverse Rapid traverse constant inclination multi-step Acceleration Speed constant inclination acceleration/deceleration multi-step acceleration/ deceleration S-pattern filter Manual rapid traverse (linear) Manual rapid traverse (linear) Soft acceleration/deceleration Time Speed (2) Rapid traverse constant inclination multi-step acceleration/deceleration cannot be used in part system excluding 1st part system. -
Page 143: Exact Stop Check; G09
7. Feed Functions 7.9 Exact Stop Check; G09 7.9 Exact Stop Check; G09 Function and purpose In order to prevent roundness during corner cutting and machine shock when the tool feedrate changes suddenly, there are times when it is desirable to start the commands in the following block once the in-position state after the machine has decelerated and stopped or the elapsing of the deceleration check time has been checked.
-
Page 144
7. Feed Functions 7.9 Exact Stop Check; G09 Detailed description (1) With continuous cutting feed Next block Previous block Fig. 2 Continuous cutting feed command (2) With cutting feed in-position check Next block Previous block Lc (in-position width) Fig. 3 Block joint with cutting feed in-position check In Figs. -
Page 145
7. Feed Functions 7.9 Exact Stop Check; G09 (3) With deceleration check (a) With linear acceleration/deceleration Next block Previous block Ts : Acceleration/deceleration time constant Td : Deceleration check time Td = Ts + ( 0 ~ 14ms) (b) With exponential acceleration/deceleration Previous block Next block Ts : Acceleration/deceleration time constant… -
Page 146: Exact Stop Check Mode; G61
7. Feed Functions 7.10 Exact Stop Check Mode; G61 7.10 Exact Stop Check Mode; G61 Function and purpose Whereas the G09 exact stop check command checks the in-position status only for the block in which the command has been assigned, the G61 command functions as a modal. This means that deceleration will apply at the end points of each block to all the cutting commands (G01 to G03) subsequent to G61 and that the in-position status will be checked.
-
Page 147
7. Feed Functions 7.11 Deceleration Check (2) Designating deceleration check The deceleration check by designating a parameter includes «deceleration check specification type 1» and «deceleration check specification type 2». The setting is selected with the parameter «#1306 InpsTyp». (a) Deceleration check specification type 1 («#1306 InpsTyp» = 0) The G0 and G1 deceleration check method can be selected with the base specification parameter deceleration check method 1 (#1193 inpos) and «deceleration check method 2″… -
Page 148: G1 -> G0 Deceleration Check
7. Feed Functions 7.11 Deceleration Check 7.11.1 G1 → G0 Deceleration Check Detailed operations (1) In G1 → G0 continuous blocks, the parameter «#1502 G0Ipfg» can be changed to change the deceleration check in the reverse direction. Same direction Reverse direction G0Ipfg: 0 G0Ipfg: 1 Command deceleration…
-
Page 149: G1 -> G1 Deceleration Check
7. Feed Functions 7.11 Deceleration Check 7.11.2 G1 → G1 Deceleration Check Detailed operations (1) In G1 → G1 continuous blocks, the parameter «#1503 G1Ipfg» can be changed to change the deceleration check of the reverse direction. Same direction Reverse direction G1Ipfg: 0 G1Ipfg: 1 Command deceleration…
-
Page 150: Automatic Corner Override
7. Feed Functions 7.12 Automatic Corner Override 7.12 Automatic Corner Override Function and purpose With tool radius compensation, this function reduces the load during inside cutting of automatic corner R, or during inside corner cutting, by automatically applying override to the feed rate. Automatic corner override is valid until the tool radius compensation cancel (G40), exact stop check mode (G61), high-accuracy control mode (G61.1), tapping mode (G63), or cutting mode (G64) command is issued.
-
Page 151
7. Feed Functions 7.12 Automatic Corner Override (1) Operation (a) When automatic corner override is not to be applied : When the tool moves in the order of (1) → (2) → (3) in Fig. 1, the machining allowance at (3) increases by an amount equivalent to the area of shaded section S and so the tool load increases. -
Page 152
7. Feed Functions 7.12 Automatic Corner Override Example of operations (1) Line — line corner Program θ Tool center Tool The override set in the parameter is applied at Ci. (2) Line — arc (outside) corner Tool center Program θ Tool The override set in the parameter is applied at Ci. -
Page 153
7. Feed Functions 7.12 Automatic Corner Override Relation with other functions Function Override at corner Cutting feed override Automatic corner override is applied after cutting feed override has been applied. Override cancel Automatic corner override is not canceled by override cancel. Speed clamp Valid after automatic corner override Dry run… -
Page 154
7. Feed Functions 7.12 Automatic Corner Override Precautions (1) Automatic corner override is valid only in the G01, G02, and G03 modes; it is not effective in the G00 mode. When switching from the G00 mode to the G01 (or G02 or G03) mode at a corner (or vice versa), automatic corner override will not be applied at that corner in the G00 block. -
Page 155: Tapping Mode; G63
7. Feed Functions 7.13 Tapping Mode; G63 7.13 Tapping Mode; G63 Function and purpose The G63 command allows the control mode best suited for tapping to be entered, as indicated below : (1) Cutting override is fixed at 100%. (2) Deceleration commands at joints between blocks are invalid. (3) Feed hold is invalid.
-
Page 156: Dwell
8. Dwell 8.1 Per-second Dwell 8. Dwell The G04 command can delay the start of the next block. 8.1 Per-second Dwell ; G04 Function and purpose The machine movement is temporarily stopped by the program command to make the waiting time state.
-
Page 157
8. Dwell 8.1 Per-second Dwell Example of program Dwell time [sec] #1078 Decpt2 = 0 #1078 Decpt2 = 1 Command DECIMAL DECIMAL DECIMAL DECIMAL PNT-N PNT-P PNT-N PNT-P G04 X500 ; G04 X5000 ; 5000 G04 X5. ; G04 X#100 ; 1000 1000 G04 P5000 ;… -
Page 158: Miscellaneous Functions
9. Miscellaneous Functions 9.1 Miscellaneous Functions (M8-digits BCD) 9. Miscellaneous Functions 9.1 Miscellaneous Functions (M8-digits BCD) Function and purpose The miscellaneous (M) functions are also known as auxiliary functions, and they include such numerically controlled machine functions as spindle forward and reverse rotation, operation stop and coolant ON/OFF.
-
Page 159
9. Miscellaneous Functions 9.1 Miscellaneous Functions (M8-digits BCD) Optional stop ; M01 If the tape reader reads the M01 command when the optional stop switch on the machine operation board is ON, it will stop and the same effect as with the M00 function will apply. If the optional stop switch is OFF, the M01 command is ignored. -
Page 160: Secondary Miscellaneous Functions (B8-Digits, A8 Or C8-Digits)
9. Miscellaneous Functions 9.2 Secondary Miscellaneous Functions (B8-digits, A8 or C8-digits) 9.2 Secondary Miscellaneous Functions (B8-digits, A8 or C8-digits) Function and purpose These serve to assign the indexing table positioning and other such functions. In this controller, they are assigned by an 8-digit number from 0 to 99999999 following address A, B or C. The machine maker determines which codes correspond to which positions.
-
Page 161: Index Table Indexing
9. Miscellaneous Functions 9.3 Index Table Indexing 9.3 Index Table Indexing Function and purpose Index table indexing can be carried out by setting the index axis. The indexing command only issues the indexing angle to the axis set for indexing. It is not necessary to command special M codes for table clamping and unclamping, thus simplifying the program.
-
Page 162
9. Miscellaneous Functions 9.3 Index Table Indexing Precautions (1) Several axes can be set as index table indexing axes. (2) The movement speed of index table indexing axes follows the feedrate of the modal (G0/G1) at that time. (3) The unclamp process for the indexing axes is also issued when the index table indexing axes are commanded in the same block as other axes. -
Page 163: Spindle Functions
10. Spindle Functions 10.1 Spindle Functions (S6-digits Analog) 10. Spindle Functions 10.1 Spindle Functions (S6-digits Analog) Function and purpose When the S6-digits function is added, a 6-digit value (0 to 999999) can be designated after the S code. Always select S command binary output when using this function. If the S function is designated in the same block as a movement command, the commands may be executed in either of the following two orders.
-
Page 164: Constant Surface Speed Control; G96, G97
10. Spindle Functions 10.3 Constant Surface Speed Control; G96, G97 10.3 Constant Surface Speed Control; G96, G97 10.3.1 Constant Surface Speed Control Function and purpose These cinommands automatically control the spindle speed in line with the changes in the radius coordinate values as cutting proceeds in the diametrical direction, and they serve to keep the cutting pot speed constant during the cutting.
-
Page 165: Spindle Clamp Speed Setting; G92
10. Spindle Functions 10.4 Spindle Clamp Speed Setting; G92 10.4 Spindle Clamp Speed Setting; G92 Function and purpose The maximum clamp speed of the spindle can be assigned by address S following G92 and the minimum clamp speed by address Q. Command format G92 S__ Q__;…
-
Page 166: Spindle/C Axis Control
10. Spindle Functions 10.5 Spindle/C Axis Control 10.5 Spindle/C Axis Control Function and purpose This function enables one spindle (MDS-A/B-SP and later) to also be used as a C axis (rotation axis) by an external signal. Detailed description (1) Spindle/C axis changeover Changeover between the spindle and C axis is done by the C axis SERVO ON signal.
-
Page 167
10. Spindle Functions 10.5 Spindle/C Axis Control (Note) For axis commands, the reference position return complete is checked at calculation. Thus, when the C axis servo ON command and C axis command are continuous, the program error (P430) occur as shown above in ∗ 2. In response to this kind of situation, the following two processes must be carried out on user PLC, as shown above in ∗… -
Page 168
10. Spindle Functions 10.5 Spindle/C Axis Control Precautions and Restrictions (1) A reference position return cannot be executed by the orientation when there is no Z phase in the detector (PLG, ENC, other). Replace the detector with one having a Z phase, or if using the detector as it is, set the position control changeover to «After deceleration stop»… -
Page 169: Multiple Spindle Control
10. Spindle Functions 10.6 Multiple Spindle Control 10.6 Multiple Spindle Control Function and purpose Multiple spindle control is a function used to control the sub-spindle in a machine tool that has a main spindle (1st spindle) and a sub-spindle (2nd spindle to 4th spindle). Multiple spindle control II: Control following the external signal (spindle (ext36/bit0 = 1)
-
Page 170: Multiple Spindle Control Ii
10. Spindle Functions 10.6 Multiple Spindle Control 10.6.1 Multiple Spindle Control II Function and purpose Multiple spindle control II is a function that designates which spindle to select with the signals from PLC. The command is issued to the spindle with one S command. Detailed description (1) Spindle command selection, spindle selection The S command to the spindle is output as the rotation speed command to the selected spindle…
-
Page 171
10. Spindle Functions 10.6 Multiple Spindle Control Relation with other functions (1) Spindle clamp speed setting (G92) This is valid only on the spindle selected with the spindle selection signal (SWS). The spindle not selected with the spindle selection signal (SWS) maintains the speed at which it was rotating at before being canceled. -
Page 172: Tool Functions (T Command)
11. Tool Functions (T command) 11.1 Tool Functions (T8-digit BCD) 11. Tool Functions (T command) 11.1 Tool Functions (T8-digit BCD) Function and purpose The tool functions are also known simply as T functions and they assign the tool numbers and tool offset number.
-
Page 173: Tool Compensation Functions
12. Tool Compensation Functions 12.1 Tool Compensation 12. Tool Compensation Functions 12.1 Tool Compensation Function and purpose The basic tool compensation function includes the tool length compensation and tool radius compensation. Each compensation amount is designated with the tool compensation No. Each compensation amount is input from the setting and display unit or the program.
-
Page 174
12. Tool Compensation Functions 12.1 Tool Compensation Tool compensation memory There are two types of tool compensation memories for setting and selecting the tool compensation amount. (The type used is determined by the machine maker specifications.) The compensation amount settings are preset with the setting and display unit. Type 1 is selected when parameter «#1037 cmdtyp»… -
Page 175
12. Tool Compensation Functions 12.1 Tool Compensation Type 1 One compensation amount corresponds to one compensation No. as shown on the right. Thus, these can be used commonly regardless of the tool length compensation amount, tool radius compensation amount, shape compensation amount and wear compensation amount. (D1) = a , (H1) = a (D2) = a… -
Page 176
12. Tool Compensation Functions 12.1 Tool Compensation Tool compensation No. (H/D) This address designates the tool compensation No. (1) H is used for the tool length compensation, and D is used for the tool position offset and tool radius compensation. (2) The tool compensation No. -
Page 177: Tool Length Compensation/Cancel; G43/G44
12. Tool Compensation Functions 12.2 Tool Length Compensation/Cancel; G43/G44 12.2 Tool Length Compensation/Cancel; G43/G44 Function and purpose The end position of the movement command can be compensation by the preset amount when this command is used. A continuity can be applied to the program by setting the actual deviation from the tool length value decided during programming as the compensation amount using this function.
-
Page 178
12. Tool Compensation Functions 12.2 Tool Length Compensation/Cancel; G43/G44 (2) Compensation No. (a) The compensation amount differs according to the compensation type. Type 1 G43 Hh When the above is commanded, the compensation amount lh commanded with compensation No. h will be applied commonly regardless of the tool length compensation amount, tool radius… -
Page 179
12. Tool Compensation Functions 12.2 Tool Length Compensation/Cancel; G43/G44 (3) Axis valid for tool length compensation (a) When parameter «#1080 Dril_Z» is set to «1», the tool length compensation is always applied on the Z axis. (b) When parameter «#1080 Dril_Z» is set to «0», the axis will depend on the axis address commanded in the same block as G43. -
Page 180: Tool Length Compensation In The Tool Axis Direction ; G43.1/G44
12. Tool Compensation Functions 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G44 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G44 Function and purpose (1) Changes in the tool length compensation in the tool axis direction and compensation amount The tool length can be compensated in the tool axis direction even when the rotation axis rotates and the tool axis direction becomes other than the Z axis direction.
-
Page 181
12. Tool Compensation Functions 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G44 Detailed description (1) G43 and G43.1 are all G codes in the same group. Therefore, it is not possible to designate more than one of these commands simultaneously for compensation. G44 is used to cancel the G43 and G43.1 commands. -
Page 182
12. Tool Compensation Functions 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G44 (Example) When changing compensation amount during single block stop. Changed compensation Changed amount compensation Path after amount compensation Compensation amount before change Program path Workpiece Single block stop (Note 3) When changing compensation amount, the compensation amount corresponding to the actual compensation No. -
Page 183
12. Tool Compensation Functions 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G44 (3) Rotary axis angle command The value used for the angle of the rotary axis (tool tip axis) differs according to the type of rotary axis involved. When servo axes are used: The machine coordinate position is used for the rotation angles of the A, B and C axes. -
Page 184
12. Tool Compensation Functions 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G44 Example of program (1) Example of arc machining Shown below is an example of a program for linear → arc → arc → linear machining using the B and C rotary axes on the ZX plane. -
Page 185
12. Tool Compensation Functions 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G44 Relation with other functions (1) Relation with 3-dimensional coordinate conversion (a) A program error (P931) will occur if 3-dimensional coordinate conversion is carried out during tool length compensation in the tool axis direction. (b) A program error (P921) will occur if the tool length is compensated in the tool axis direction during 3-dimensional coordinate conversion. -
Page 186
12. Tool Compensation Functions 12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G44 (b) Reference position return for the rotary axis Tool length compensation in the tool axis direction will be canceled, as well as the dog-type reference position return and the high-speed reference position return. <A axis Manual reference position return>… -
Page 187: Tool Radius Compensation; G38, G39/G40/G41,G42
12. Tool Compensation Functions 12.4 Tool Radius Compensation 12.4 Tool Radius Compensation; G38, G39/G40/G41,G42 Function and purpose This function compensates the radius of the tool. The compensation can be done in the random vector direction by the radius amount of the tool selected with the G command (G38 to G42) and the D command.
-
Page 188: Tool Radius Compensation Operation
12. Tool Compensation Functions 12.4 Tool Radius Compensation 12.4.1 Tool Radius Compensation Operation Tool radius compensation cancel mode The tool radius compensation cancel mode is established by any of the following conditions. (1) After the power has been switched on (2) After the reset button on the setting and display unit has been pressed (3) After the M02 or M30 command with reset function has been executed (4) After the tool radius compensation cancel command (G40) has been executed…
-
Page 189
12. Tool Compensation Functions 12.4 Tool Radius Compensation Start of movement for tool radius compensation (1) For inner side of corner Linear Circular Linear Linear θ θ Program path Program r = Compensation amount path Tool center path Tool center path Start point Start point… -
Page 190
12. Tool Compensation Functions 12.4 Tool Radius Compensation (3) For outer side of corner (obtuse angle) [0<90°] Linear Linear(Type A) Linear Circular(Type A) Center of circular Tool center path Program path Tool center path θ θ Program path Start point Start point Linear Circular(Type B) -
Page 191
12. Tool Compensation Functions 12.4 Tool Radius Compensation Operation in compensation mode Relative to the program path (G00, G01, G02, G03), the tool center path is found from the straight line/circular arc to make compensation. Even if the same compensation command (G41, G42) is issued in the compensation mode, the command will be ignored. -
Page 192
12. Tool Compensation Functions 12.4 Tool Radius Compensation Circular Linear (90°≤θ<180°) Circular Linear (0°<θ<90°) Center of circular Program path Program path θ θ Tool center path Tool center path Center of circular Point of intersection Circular Circular (90°≤θ<180°) Circular Circular (0°<θ<90°) Center of circular Program path θ… -
Page 193
12. Tool Compensation Functions 12.4 Tool Radius Compensation (2) Machining an inner wall Linear Linear (Acute angle) Linear Linear (Obtuse angle) θ θ Program path Program path Tool center path Tool center path Point of intersection Linear Circular (Acute angle) Linear Circular (Obtuse angle) θ… -
Page 194
12. Tool Compensation Functions 12.4 Tool Radius Compensation (3) When the arc end point is not on the arc For spiral arc ……A spiral arc will be interpolated from the start to end point of the arc. For normal arc command..If the error after compensation is within parameter «#1084 RadErr», the area from the arc start point to the end point is interpolated as a spiral arc. -
Page 195
12. Tool Compensation Functions 12.4 Tool Radius Compensation Tool radius compensation cancel operation (1) For inner side of corner Linear Linear Circular Linear θ θ Program path r = Compensation amount Program path Tool center path Tool center path End point End point Center of circular (2) For outer side of corner (obtuse angle) -
Page 196
12. Tool Compensation Functions 12.4 Tool Radius Compensation (3) For outer side of corner (acute angle) Circular Linear (Type A) Linear Linear (Type A) Center of circular Tool center path Tool center path Program path θ Program path θ End point End point Circular Linear (Type B) -
Page 197: Other Commands And Operations During Tool Radius Compensation
12. Tool Compensation Functions 12.4 Tool Radius Compensation 12.4.2 Other Commands and Operations During Tool Radius Compensation Insertion of corner arc An arc that uses the compensation amount as the radius is inserted without calculating the point of intersection at the workpiece corner when G39 (corner arc) is commanded. Point of Inserted intersection…
-
Page 198
12. Tool Compensation Functions 12.4 Tool Radius Compensation Changing and holding of compensation vector The compensation vector can be changed or held during tool radius compensation by using the G38 command. (1) Holding of vector: When G38 is commanded in a block having a movement command, the point of intersection will not be calculated at the program end point, and instead the vector of the previous block will be held. -
Page 199
12. Tool Compensation Functions 12.4 Tool Radius Compensation Changing the compensation direction during tool radius compensation The compensation direction is determined by the tool radius compensation commands (G41, G42) and compensation amount sign. Compensation amount sign G code Left-hand compensation Right-hand compensation Right-hand compensation Left-hand compensation… -
Page 200
12. Tool Compensation Functions 12.4 Tool Radius Compensation Circular → Circular Tool center path Circular center ‚’ ’ Program path ‚’ ’ Circular center Linear return Tool center path Program path In the case below, it is possible that the arc Arc exceeding 360°… -
Page 201
12. Tool Compensation Functions 12.4 Tool Radius Compensation Command for eliminating compensation vectors temporarily When the following command is issued in the compensation mode, the offset vectors are temporarily eliminated and a return is then made automatically to the compensation mode. In this case, the compensation is not canceled, and the tool goes directly from the intersection point vector to the point without vectors or, in other words, to the programmed command point. -
Page 202
12. Tool Compensation Functions 12.4 Tool Radius Compensation Blocks without movement and pre-read inhibit M command The following blocks are known as blocks without movement. a. M03 ; ………M command b. S12 ; ……..S command c. T45 ; ……..T command d. -
Page 203
12. Tool Compensation Functions 12.4 Tool Radius Compensation (2) When command is assigned in the compensation mode When 4 or more blocks without movement follow in succession in the compensation mode or when there is no pre-read inhibit M code, the intersection point vectors will be created as usual. -
Page 204
12. Tool Compensation Functions 12.4 Tool Radius Compensation When I, J, K are commanded in G40 (1) If the final movement command block in the four blocks before the G40 block is the G41 or G42 mode, it will be assumed that the movement is commanded in the vector I, J or K direction from the end point of the final movement command. -
Page 205
12. Tool Compensation Functions 12.4 Tool Radius Compensation (2) If the arc is 360° or more due to the details of I, J and K at G40 after the arc command, an uncut section will occur. Uncut section N1 (G42,G91) G01X200. ; (i,j) N2 G02 J150. -
Page 206: G41/G42 Commands And I, J, K Designation
12. Tool Compensation Functions 12.4 Tool Radius Compensation 12.4.3 G41/G42 Commands and I, J, K Designation Function and purpose The compensation direction can be intentionally changed by issuing the G41/G42 command and I, J, K in the same block. Command format G17 (XY plane) G41/G42 X__ Y__ I__ J__ ;…
-
Page 207
12. Tool Compensation Functions 12.4 Tool Radius Compensation (3) When I, J has been commanded in the G41/G42 mode (G17 plane) (I,J)N110 (G17 G41 G91) N100 N100 G41 G00X150. J50. ; N120 N110 G02 I150. ; N120 G00 X−150. ; (N120) (1) I, J type vector (2) Intersection point calculation… -
Page 208
12. Tool Compensation Functions 12.4 Tool Radius Compensation (4) When I, J has been commanded in a block without movement N1 G41 D1 G01 F1000 ; (I,J) N2 G91 X100. Y100. ; N3 G41 I50. ; N4 X150. ; N5 G40 ; Direction of compensation vectors (1) In G41 mode Direction produced by rotating the direction commanded by I, J through 90°… -
Page 209
12. Tool Compensation Functions 12.4 Tool Radius Compensation Selection of compensation modal The G41 or G42 modal can be selected at any time. N1 G28 X0 Y0 ; N2 G41 D1 F1000 ; N3 G01 G91 X100. Y100. ; N4 G42 X100. I100. J-100. D2 ; (I,J) N5 X100. -
Page 210
12. Tool Compensation Functions 12.4 Tool Radius Compensation Precautions (1) Issue the I, J type vector in a linear mode (G0, G1). If it is issued in an arc mode at the start of compensation, program error (P151) will occur. An IJ designation in an arc mode functions as an arc center designation in the compensation mode. -
Page 211
12. Tool Compensation Functions 12.4 Tool Radius Compensation (4) Refer to the following table for the offset methods based on the presence and/or absence of the G41 and G42 commands and I, J, (K) command. G41/G42 I, J (K) Offset method Intersection point calculation type vector Intersection point calculation type vector Intersection point calculation type vector… -
Page 212: Interrupts During Tool Radius Compensation
12. Tool Compensation Functions 12.4 Tool Radius Compensation 12.4.4 Interrupts During Tool Radius Compensation MDI interrupt Tool radius compensation is valid in any automatic operation mode-whether tape, memory or MDI operation. An interrupt based on MDI will give the result as in the figure below after block stop during tape or memory operation.
-
Page 213
12. Tool Compensation Functions 12.4 Tool Radius Compensation Manual interrupt (1) Interrupt with manual absolute OFF. Tool path after interrupt The tool path is shifted by an amount equivalent to the interrupt amount. Tool path after Interrupt compensation Program path (2) Interrupt with manual absolute ON. -
Page 214: General Precautions For Tool Radius Compensation
12. Tool Compensation Functions 12.4 Tool Radius Compensation 12.4.5 General Precautions for Tool Radius Compensation Precautions (1) Designating the offset amounts The offset amounts can be designated with the D code by designating an offset amount No. Once designated, the D code is valid until another D code is commanded. If an H code is designated, the program error (P170) No COMP No will occur.
-
Page 215: Changing Of Compensation No. During Compensation Mode
12. Tool Compensation Functions 12.4 Tool Radius Compensation 12.4.6 Changing of Compensation No. During Compensation Mode Function and purpose As a principle, the compensation No. must not be changed during the compensation mode. If changed, the movement will be as shown below. When offset No.
-
Page 216
12. Tool Compensation Functions 12.4 Tool Radius Compensation (2) Linear circular Tool center path N102 Program path N101 Tool center path Center of circular Program path N101 N102 Center of circular (3) Circular circular Tool center path Program path N101 N102 Center of circular Center of circular… -
Page 217: Start Of Tool Radius Compensation And Z Axis Cut In Operation
12. Tool Compensation Functions 12.4 Tool Radius Compensation 12.4.7 Start of Tool Radius Compensation and Z Axis Cut in Operation Function and purpose Often when starting cutting, a method of applying a radius compensation (normally the XY plane) beforehand at a position separated for the workpiece, and then cutting in with the Z axis is often used.
-
Page 218
12. Tool Compensation Functions 12.4 Tool Radius Compensation In this case, consider the calculation of the inner side, and before the Z axis cutting, issue a command in the same direction as the direction that the Z axis advances in after lowering, to prevent excessive cutting. -
Page 219: Interference Check
12. Tool Compensation Functions 12.4 Tool Radius Compensation 12.4.8 Interference Check Function and purpose (1) Outline A tool, whose radius has been compensated with the tool radius compensation function by the usual 2-block pre-read, may sometimes cut into the workpiece. This is known as interference, and interference check is the function which prevents this from occurring.
-
Page 220
12. Tool Compensation Functions 12.4 Tool Radius Compensation (3) With interference check invalid function The tool passes while cutting the N1 and N3 line. (4)’ (3)’ (2)’ (1)’ Example of interference check → No interference Vectors (1) (4)’ check ↓ →… -
Page 221
12. Tool Compensation Functions 12.4 Tool Radius Compensation Conditions viewed as interference If there is a movement command in three of the five pre-read blocks, and if the compensation calculation vectors created at the contacts of each movement command intersect, it will be viewed as interference. -
Page 222
12. Tool Compensation Functions 12.4 Tool Radius Compensation Operation during interference avoidance The movement will be as shown below when the interference avoidance check is used. Tool center path Program path Solid line vector : Valid Tool center path when interference is avoided Dotted line vector : Invalid Tool center path without interference check Program path… -
Page 223
12. Tool Compensation Functions 12.4 Tool Radius Compensation Avoidance vector Tool center path Avoidance vector Program path If all of the line vectors for the interference avoidance are deleted, create a new avoidance vector as shown on the right to avoid the interference. -
Page 224
12. Tool Compensation Functions 12.4 Tool Radius Compensation Interference check alarm The interference check alarm occurs under the following conditions. (1) When the interference check alarm function has been selected (a) When all the vectors at the end block of its own block have been deleted. When, as shown in the figure, vectors 1 through 4 at the end point of the N1 block have all… -
Page 225
12. Tool Compensation Functions 12.4 Tool Radius Compensation (b) When avoidance vectors cannot be created Even when, as in the figure, the conditions for Alarm stop creating the avoidance vectors are met, it may still be impossible to create these vectors or the interference vectors may interfere with N3. -
Page 226: Diameter Designation Of Compensation Amount
12. Tool Compensation Functions 12.4 Tool Radius Compensation 12.4.9 Diameter Designation of Compensation Amount Function and purpose With this function, the tool radius compensation amount can be designated by tool diameter. When the control parameter “#8117 OFS Diam DESIGN” is ON, the compensation amount specified to the commanded tool No.
-
Page 227
12. Tool Compensation Functions 12.4 Tool Radius Compensation (b) Linear to arc (obtuse angle) Outside of the corner Inside of the corner θ θ Program path Program path Tool center path (When #8117 is ON) Tool center path Arc center (When #8117 is OFF) Arc center (c) Arc to linear (obtuse angle) -
Page 228: Workpiece Coordinate Changing During Radius Compensation
12. Tool Compensation Functions 12.4 Tool Radius Compensation 12.4.10 Workpiece Coordinate Changing During Radius Compensation Function and purpose When the tool radius compensation is executed, the tool center path is calculated based on the position on the coordinate system. The based coordinate system can be changed by the parameter.
-
Page 229
12. Tool Compensation Functions 12.4 Tool Radius Compensation The coordinate system changed by parameter is as follows. G90 G54 G00 X15. Y20. N1 G41 D3 X5. Y10.; N2 G01 Y-20. F1000; N3 G40 X30.; M30; D3 = 5.000 G54 offset X15.000 Y15.000 (i) Parameter = 0… -
Page 230: Three-Dimensional Tool Radius Compensation ; G40/G41,G42
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42 Function and purpose The three-dimensional tool radius compensation compensates the tool in a three-dimensional space following the commanded three-dimensional vectors. Tool Tool center coordinate position Plane normal line vector…
-
Page 231
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42 Command format Command the compensation No. D and plane normal line vector (I, J, K) in the same block as the three-dimensional tool radius compensation command G41 (G42). If only one or two axes are commanded, the normal tool radius compensation mode will be applied. (When setting «0»… -
Page 232
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42 Example of operation (1) Compensation start: When there is a movement command G41 xx Yy Zz Ii Jj Kk Dd ; Tool center path Three-dimensional compensation vector Program path Start point (2) Compensation start: When there is no movement command G41 Ii Jj Kk Dd ;… -
Page 233
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42 (5) Movement during the compensation: For arc or helical cutting The I, J, K commands for a circular or helical cutting are regarded as the circular center commands, thus, the new vector is equivalent to the old vector. Even for the R-designation method, commanded I, J, K addresses will be ignored, then the new vector will be equivalent to the old vector. -
Page 234
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42 (7) Movement during the compensation: When compensation direction is to be changed G41 Xx Yy Zz Ii Jj Kk Dd1 ; New vector G42 Xx Yy Zz Ii Jj Kk ; Tool center path Old vector… -
Page 235
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42 Relation with other functions (1) Normal tool radius compensation If the plane normal line vector (I, J, K) is not commanded for all three axes in the three-dimensional tool radius compensation start block, the normal tool radius compensation mode will take place. -
Page 236
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42 (6) Program coordinate rotation Program coordinate rotation is executed in respect to the coordinates before three-dimensional tool radius compensation. The plane normal line vector (I, J, K) dose not rotate. D1=10. -
Page 237
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42 (12) Machine coordinate system selection (a) For the absolute command, all axes will be temporarily canceled at the commanded coordinate position. D1=10. -50. -30. -20. -10. G90 ; N1 G41 D1 X-10. Y-20. Z-10. I-5. Program path J-5. -
Page 238
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42 (13) Coordinate system setting When commanded in the same block as the coordinate system setting, the coordinate system will be set, and operation will start up independently with the plane normal line vector (I, J, K). -
Page 239
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42 (14) Reference position return All the axes will be temporarily canceled at the intermediate point. D1=10. -70. -50. -30. -20. G91 ; M(0,0) N1 G41 D1 X-10. Y-20. Z-10. I-5. -50. -
Page 240
12. Tool Compensation Functions 12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42 Restrictions (1) The compensation No. is selected with the D address, however, the D address is valid only when G41 or G42 is commanded. If D is not commanded, the number of the previous D address will be valid. -
Page 241: Tool Position Offset; G45 To G48
12. Tool Compensation Functions 12.6 Tool Position Offset; G45 to G48 12.6 Tool Position Offset; G45 to G48 Function and purpose Using the G45 to G46 commands, the movement distance of the axes specified in the same block can be extended or reduced by a preset compensation length. Furthermore, the compensation amount can be similarly doubled (x 2 expansion) or halved (x 2 reduction) with commands G47 and G48.
-
Page 242
12. Tool Compensation Functions 12.6 Tool Position Offset; G45 to G48 Detailed description Details for incremental values are given below. Movement amount of equivalent command Example Command (assigned compensation (when X = 1000) amount = l) l = 10 1010 G45Xx Dd X ( x + l ) l = −10… -
Page 243
12. Tool Compensation Functions 12.6 Tool Position Offset; G45 to G48 (4) In the case of circular interpolation, cutter compensation is possible using the G45 to G48 commands only for one quadrant, two quadrants (semi-sphere) or three quadrants when the start and end points are on the axis. -
Page 244
12. Tool Compensation Functions 12.6 Tool Position Offset; G45 to G48 Example of program (Example 1) End point Tool nose center path Programmed 1000 path Tool Start point 1000 Programmed arc center Tool position offset with 1/4 arc command It is assumed that compensation has already been provided in the + X direction by D01 = 200. -
Page 245
12. Tool Compensation Functions 12.6 Tool Position Offset; G45 to G48 When a command for «n» number of simultaneous axes is given, the same compensation will be applied to all axes. It is valid even for the additional axes (but it must be within the range of the number of axes which can be controlled simultaneously.) G01 G45X220. -
Page 246
12. Tool Compensation Functions 12.6 Tool Position Offset; G45 to G48 (Example 2) Tool nose center path N1 G46 G00 Xx1 Yy1 Dd1 ; N2 G45 G01 Yy2 Ff2 ; N3 G45 G03 Xx3 Yy3 Ii3 ; N4 G01 Xx4 ; Programmed path (Example 3) When the G45 to G48 command is assigned, the compensation amount for each pass… -
Page 247
12. Tool Compensation Functions 12.6 Tool Position Offset; G45 to G48 Compensation amount D01 = 10.000mm (Offset amount of tool radius) N100 X40.0 Y40.0 D01 ; N101 X100.0 F200 N102 X10.0 Y10.0 J10.0 ; N103 Y40.0 N104 N105 X−20.0 Y20.0 J20.0 ;… -
Page 248: Programmed Compensation Input; G10, G11.1
12. Tool Compensation Functions 12.7 Programmed Compensation Input; G10, G11.1 12.7 Programmed Compensation Input; G10, G11.1 Function and purpose The tool compensation and workpiece offset can be set or changed on the tape using the G10 command. During the absolute value (G90) mode, the commanded compensation amount will become the new compensation amount, and during the incremental value (G91) mode, the commanded compensation amount will be added to the currently set compensation amount to create the new compensation amount.
-
Page 249
12. Tool Compensation Functions 12.7 Programmed Compensation Input; G10, G11.1 Detailed description (1) Program error (P171) will occur if this command is input when the specifications are not available. (2) G10 is an unmodal command and is valid only in the commanded block. (3) The G10 command does not contain movement, but must not be used with G commands other than G54 to G59, G90 or G91. -
Page 250
12. Tool Compensation Functions 12.7 Programmed Compensation Input; G10, G11.1 (Example 2) Assume that H10 = -1000 is already set. Main program G00 X100000 ; #1 = -1000 ; G22 L1111 L4 ; Subprogram L1111 G01 G91 G43 Z0 H10 F100 ; G01 X1000 ;… -
Page 251
12. Tool Compensation Functions 12.7 Programmed Compensation Input; G10, G11.1 (3) When updating the workpiece coordinate system offset amount Assume that the previous workpiece coordinate system offset amount is as follows. X = −10.000 Y = −10.000 N100 G00 G90 G54 X0 Y0 ; N101 G90 G10 L2 P1 X−15.000 Y−15.000 ;… -
Page 252
12. Tool Compensation Functions 12.7 Programmed Compensation Input; G10, G11.1 (4) When using one workpiece coordinate system as multiple workpiece coordinate systems #1 = −50. #2 = 10. ; L200 P5 ; Main program M02 ; G90 G54 G10 L2 P1 X#1 Y#1 ; G00 X0 Y0 ;… -
Page 253: Compensation Data Input To Variable By Program; G11
12. Tool Compensation Functions 12.8 Compensation Data Input to Variable by Program; G11 12.8 Compensation Data Input to Variable by Program; G11 Function and purpose Using G11, the compensation amount of the No. commanded as the transmission source can be set into the arbitrary variable.
-
Page 254: Inputting The Tool Life Management Data; G10, G11
12. Tool Compensation Functions 12.9 Inputting the Tool Life Management Data; G10, G11 12.9 Inputting the Tool Life Management Data; G10, G11 12.9.1 Inputting the Tool Life Management Data by G10 L3 Command Function and purpose Using the G10 command (unmodal command), the tool life management data can be registered, changed and added to, and preregistered groups can be deleted.
-
Page 255
12. Tool Compensation Functions 12.9 Inputting the Tool Life Management Data; G10, G11 Example of operation Program example Operation Data G10 L3; 1. After deleting all group data, the registration starts. registration P10 L10 Q1; 2. Group No. 10 is registered. T10 H10 D10;… -
Page 256: Inputting The Tool Life Management Data By G10 L30 Command
12. Tool Compensation Functions 12.9 Inputting the Tool Life Management Data; G10, G11 12.9.2 Inputting the Tool Life Management Data by G10 L30 Command Function and purpose Using the G10 command (unmodal command), the tool life management data can be registered, changed and added to, and preregistered groups can be deleted.
-
Page 257
12. Tool Compensation Functions 12.9 Inputting the Tool Life Management Data; G10, G11 (3) Deleting a group G10 L30 P2; Start of life management data deletion Delete the group No. Delete next group No. G11 ; End life management data deletion : Group No. -
Page 258
12. Tool Compensation Functions 12.9 Inputting the Tool Life Management Data; G10, G11 Command range Item Command range Group No. (Pn) 1 to 99999999 Tool No. (Tn) 1 to 99999999 Control method (Qabc) abc : Three integer digits a. Tool length compensation data format 0: Compensation No. -
Page 259: Precautions For Inputting The Tool Life Management Data
12. Tool Compensation Functions 12.9 Inputting the Tool Life Management Data; G10, G11 12.9.3 Precautions for Inputting the Tool Life Management Data Precautions (1) The tool life data is registered, changed, added to or deleted by executing the program in the memory or MDI mode.
-
Page 260: Fixed Cycles
13. Program Support Functions 13.1 Fixed Cycles 13. Program Support Functions 13.1 Fixed Cycles 13.1.1 Standard Fixed Cycles; G80 to G89, G73, G74, G75, G76 Function and purpose These standard canned cycles are used for predetermined sequences of machining operations such as positioning, hole drilling, boring, tapping, etc.
-
Page 261
13. Program Support Functions 13.1 Fixed Cycles Command format (1) Label L G8Δ (G7Δ) X__ Y__ Z__ R__ Q__ P__(E__) F__ L__(H__) S__ ,S__ ,I__ ,J__ ; G8Δ (G7Δ) X__ Y__ Z__ R__ Q__ P__(E__) F__ L__(H__) S__ ,R__ ,I__ ,J__ ; : Hole machining mode G8Δ… -
Page 262
13. Program Support Functions 13.1 Fixed Cycles Detailed description (1) Outline of data and corresponding addresses (a) Hole machining mode: Canned cycle modes such as drilling, counter boring, tapping and boring. (b) Hole position data: Data used to position the X and Y axes. (Unmodal) (c) Hole machining data: Actual machining data used for machining. -
Page 263
13. Program Support Functions 13.1 Fixed Cycles (4) Canned cycle addresses and meanings Address Significance Label L Label O Selection of hole machining cycle sequence (G80 to G89, G73, G74, G76) Designation of hole drilling position (absolute value or incremental value) Designation of hole drilling position (absolute value or incremental value) Designation of hole bottom position (absolute value or… -
Page 264
13. Program Support Functions 13.1 Fixed Cycles (5) Difference between absolute value command and incremental value command For absolute value For incremental value R point R point Workpiece Workpiece (6) Feed rate for tapping cycle and tapping return The feed rates for the tapping cycle and tapping return are as shown below. (a) Selection of synchronous tapping cycle/asynchronous tapping cycle Control parameter Synchronous/… -
Page 265
13. Program Support Functions 13.1 Fixed Cycles (c) Spindle rotation speed during return of synchronous tapping cycle Meaning of Command Address Remarks address range (unit) Spindle 0 to 99999 The data is held as modal information. rotation If the value is smaller than the speed (r/min) speed during rotation speed, the speed rotation speed… -
Page 266
13. Program Support Functions 13.1 Fixed Cycles Programmable in-position width command in fixed cycle This command commands the in-position width for the fixed cycle from the machining program. The commanded in-position width is valid only in the G81 (drill, spot drill), G82 (drill, counter boring), G83 (deep drill cycle), G84 (tap cycle), G85 (boring), G89 (boring), G73 (step cycle) and G74 (reverse tap cycle) fixed cycles. -
Page 267
13. Program Support Functions 13.1 Fixed Cycles Operation Operation5 Operation9 Operation1 pattern -10. -10. -50. Operation 1 Valid – Opera- Opera- Operation 2 – Invalid tion10 tion6 Operation2 Operation 3 – Invalid Operation 4 – Valid Operation 5 Invalid – Opera- Opera- Operation3… -
Page 268
13. Program Support Functions 13.1 Fixed Cycles (2) Relation between the in-position width and tap axis movement for a synchronous tap in-position check (1) Section in which the in- R point Hole bottom position check is carried out by the sv024 value. (2) Section in which the in- ↑… -
Page 269
13. Program Support Functions 13.1 Fixed Cycles (3) Relation between the parameter setting values and tap axis movement for a synchronous tap in-position check #1223 aux07 Bit3 Bit4 Bit5 Bit2 Hole bottom Operation Operation Operation at Synchronous → I point R point wait time at hole bottom… -
Page 270
13. Program Support Functions 13.1 Fixed Cycles Movement when executing each fixed cycles (a) G81 (Drilling, spot drilling) Program G81 Xx1 Yy1 Zz1 Rr1 Ff1 ,Ii1 ,Jj1; (1) G0 Xx (2) G0 Zr (3) G1 Zz (4) G98 mode G0Z − (z G99 mode G0Z −… -
Page 271
13. Program Support Functions 13.1 Fixed Cycles (c) G83 (Deep hole drilling cycle) Program G83 Xx Q : This designates the cutting amount per pass, and is always designated with an incremental value. (3) (4) (10) (1) G0 Xx (2) G0 Zr (3) G1 Zq (4) G0 Z −… -
Page 272
13. Program Support Functions 13.1 Fixed Cycles (d) G84 (Tapping cycle) Program G84 Xx (or S ) ,Ii P : Dwell designation (1) G0 Xx (2) G0 Zr (3) G1 Zz (4) G4 Pp (5) M4 (Spindle reverse rotation) (7) (8) (6) G1 Z −… -
Page 273
13. Program Support Functions 13.1 Fixed Cycles This function allows spindle acceleration/deceleration pattern to be approached to the speed loop acceleration/deceleration pattern by dividing the spindle and drilling axis acceleration/deceleration pattern into up to three stages during synchronous tapping. The acceleration/deceleration pattern can be set up to three stages for each gear. When returning from the hole bottom, rapid return is possible depending on the spindle rotation speed during return. -
Page 274
13. Program Support Functions 13.1 Fixed Cycles (ii) When synchronous tap changeover spindle rotation speed 2 < spindle rotation speed during return Smax S(S1) S'(Smax) : Command spindle rotation speed : Spindle rotation speed during return : Tap rotation speed (spindle base specification parameters #3013 to #3016) : Synchronous tap changeover spindle rotation speed 2 (spindle base specification parameters #3037 to #3040) Smax : Maximum rotation speed (spindle base specification parameters #3005 to… -
Page 275
13. Program Support Functions 13.1 Fixed Cycles (e) G85 (Boring) Program G85 Xx (1) G0 Xx (2) G0 Zr (3) G1 Zz (4) G1 Z − z G98 mode G0Z − r G99 mode No movement G98 G99 mode mode Operation pattern Valid… -
Page 276
13. Program Support Functions 13.1 Fixed Cycles (g) G87 (Back boring) Program G87 Xx (Note) Take care to the z and r designations. (The z and r symbols are reversed). There is no R point return. G0 Xx M19 (Spindle orient) G0 Xq ) (Shift) (12)(11) -
Page 277
13. Program Support Functions 13.1 Fixed Cycles (h) G88 (Boring) Program G88 Xx (1) G0 Xx (2) G0 Zr (3) G1 Zz (4) G4 Pp (5) M5 (Spindle stop) (6) Stop when single block stop switch is ON. (7) Automatic start switch ON G98 mode G0Z −… -
Page 278
13. Program Support Functions 13.1 Fixed Cycles G73 (Step cycle) Program G73 Xx P : Dwell designation (1) G0 Xx (2) G0 Zr (3) G1 Zq (n) -1 (4) G4 Pp (5) G0 Z − m (6) G1 Z (q + m) Ff mode mode… -
Page 279
13. Program Support Functions 13.1 Fixed Cycles (k) G74 (Reverse tapping cycle) Program G74 Xx (or S ) ,Ii P : Dwell designation (1) G0 Xx (2) G0 Zr (3) G1 Zz (4) G4 Pp (7)(8) (5) M3 (Spindle forward rotation) (7) (8) (6) G1 Z –… -
Page 280
13. Program Support Functions 13.1 Fixed Cycles This function allows spindle acceleration/deceleration pattern to be approached to the speed loop acceleration/deceleration pattern by dividing the spindle and drilling axis acceleration/deceleration pattern into up to three stages during synchronous tapping. The acceleration/deceleration pattern can be set up to three stages for each gear. When returning from the hole bottom, rapid return is possible depending on the spindle rotation speed during return. -
Page 281
13. Program Support Functions 13.1 Fixed Cycles (ii) When synchronous tap changeover spindle rotation speed 2 < spindle rotation speed during return Smax S(S1) S'(Smax) : Command spindle rotation speed : Spindle rotation speed during return : Tap rotation speed (spindle base specification parameters #3013 to #3016) : Synchronous tap changeover spindle rotation speed 2 (spindle base specification parameters #3037 to #3040) Smax : Maximum rotation speed (spindle base specification parameters #3005 to… -
Page 282
13. Program Support Functions 13.1 Fixed Cycles (iii) Pecking tapping cycle The load applied to the tool can be reduced by designating the depth of cut per pass (Q) and cutting the workpiece to the hole bottom for a multiple number of passes. The amount retracted from the hole bottom is set to the parameter «#8018 G84/G74 return». -
Page 283
13. Program Support Functions 13.1 Fixed Cycles (iv) Deep-hole tapping cycle In the deep-hole tapping, the load applied to the tool can be reduced by designating the depth of cut per pass and cutting the workpiece to the hole bottom for a multiple number of passes. -
Page 284
13. Program Support Functions 13.1 Fixed Cycles G75 (Fine boring) Circle cutting cycle performs a series of the cutting as follows: First: positioning of X and Y axes to the circle center. Next: cutting in with Z axis to the commanded position. Then: moving the perfect round cutting the inside of the circle. -
Page 285
13. Program Support Functions 13.1 Fixed Cycles (m) G76 (Fine boring) Program G76 Xx (1) G0 Xx (2) G0 Zr (3) G1 Zz (4) M19 (Spindle orient) (5) G1 Xq ) Ff (Shift) G98 mode G0Z − (z G99 mode G0Z − z (7) G0 X −… -
Page 286
13. Program Support Functions 13.1 Fixed Cycles Precautions for using canned cycle (1) Before the canned cycle is commanded, the spindle must be rotating in a specific direction with an M command (M3 ; or M4 ;). Note that for the G87 (back boring) command, the spindle rotation command is included in the canned cycle so only the rotation speed command needs to be commanded beforehand. -
Page 287
13. Program Support Functions 13.1 Fixed Cycles (12) If the spindle rotation speed value during return is smaller than the spindle speed, the spindle rotation speed value is valid even during return. (13) If the 2nd and 3rd acceleration/deceleration stage inclinations following the spindle rotation speed and time constants set in the parameters are each steeper than the previous stage’s inclination, the previous stage’s inclination will be valid. -
Page 288: Drilling Cycle With High-Speed Retract
13. Program Support Functions 13.1 Fixed Cycles 13.1.2 Drilling Cycle with High-Speed Retract Function And Purpose This function retracts the drill from the hole bottom at high speed in drilling machining. This function helps extending the drill life by reducing the time of drilling in vain at hole bottom. <When Axis prefiltering is enabled>…
-
Page 289
13. Program Support Functions 13.1 Fixed Cycles (c) If the drilling axis is synchronously controlled, set the same value in both parameters for primary and secondary axes. (3) While G80 (Fixed cycle cancel) command is issued, this function is canceled by issuing any other fixed cycle of the same group (Group 9) or any Group 1 command. -
Page 290
13. Program Support Functions 13.1 Fixed Cycles (3) Operation of G73 command Initial point Start point G98 mode 1) Moves from start point to initial point (2) Moves from initial point to R point (3) Cutting feed G99 mode R point (4) Retracted at high-speed (5) Moves to the position set with “G73 return amount“… -
Page 291: Initial Point And R Point Level Return; G98, G99
13. Program Support Functions 13.1 Fixed Cycles 13.1.3 Initial Point and R Point Level Return; G98, G99 Function and purpose Whether to use R point or initial level for the return level in the final sequence of the canned cycle can be selected.
-
Page 292
13. Program Support Functions 13.1 Fixed Cycles Example of program (Example 1) Record only the hold machining data G82 Zz L0 ; (Do not execute) Execute hole drilling operation with G82 mode The No. of canned cycle repetitions is designated with L. If L1 is designated or L not designated, the canned cycle will be executed once. -
Page 293: Setting Of Workpiece Coordinates In Fixed Cycle Mode
13. Program Support Functions 13.1 Fixed Cycles 13.1.4 Setting of Workpiece Coordinates in Fixed Cycle Mode The designated axis moves with the workpiece coordinate system set for the axis. The Z axis is valid after the R point positioning after positioning or from Z axis movement. (Note) When the workpiece coordinates are changed over for address Z and R, re-program even if the values are the same.
-
Page 294: Special Fixed Cycle; G34, G35, G36, G37
13. Program Support Functions 13.2 Special Fixed Cycle 13.2 Special Fixed Cycle; G34, G35, G36, G37 Function and purpose The special fixed cycle is used with the standard fixed cycle. Before using the special fixed cycle, program the fixed cycle sequence selection G code and hole machining data to record the hole machining data.
-
Page 295
13. Program Support Functions 13.2 Special Fixed Cycle Bolt hole circle (G34) I r J θ K n ; G34 X x X, Y :Positioning of bolt hole cycle center. This will be affected by G90/G91. :Radius r of the circle. The unit follows the input setting unit, and is given with a positive number. -
Page 296
13. Program Support Functions 13.2 Special Fixed Cycle Line at angle (G35) G35 X x1 Y y1 I d J θ K n ; X, Y :Designation of start point coordinates. This will be affected by G90/G91. :Interval d. The unit follows the input setting unit. If d is negative, the drilling will take place in the direction symmetrical to the point that is the center of the start point. -
Page 297
13. Program Support Functions 13.2 Special Fixed Cycle Arc (G36) G36 X x1 Y y1 I r J θ P Δθ K n ; X, Y :Center coordinates of arc. This will be affected by G90/G91. :Radius r of arc. The unit follows the input setting unit, and is given with a positive :Angle θ… -
Page 298
13. Program Support Functions 13.2 Special Fixed Cycle Grid (G37) G37 X x1 Y y1 I Dx P nx J Dy K ny ; X, Y :Designation of start point coordinates. This will be affected by G90/G91. :Interval Dx of the X axis. The unit will follow the input setting unit. If Dx is positive, the interval will be in the forward direction looking from the start point, and when negative, will be in the reverse direction looking from the start point. -
Page 299: Subprogram Control; G22, G22
13. Program Support Functions 13.3 Subprogram Control 13.3 Subprogram Control; G22, G22 13.3.1 Calling Subprogram with G22 and G22 Commands Function and purpose Fixed sequences or repeatedly used parameters can be stored in the memory as subprograms which can then be called from the main program when required.G22 serves to call subprograms and G23 serves to return operation from the subprogram to the main program.
-
Page 300
13. Program Support Functions 13.3 Subprogram Control Command format Subprogram call G22 L__ H__ P__ ,D__; or G22 <File name> H__ P__ ,D__ ; Subprogram call command Program No. of subprogram to be called (own program if omitted) A (label O) L(A) address can be omitted only during memory mode and MDI mode. -
Page 301
13. Program Support Functions 13.3 Subprogram Control (2) Only those subprograms Nos. ranging from 1 to 99999999 designated by the optional specifications can be used. When there are no program Nos. on the tape, they are entered as the setting No. for «program input.» (3) Up to 8 nesting levels can be used for calling programs from subprograms, and program error (P230) results if this number is exceeded. -
Page 302
13. Program Support Functions 13.3 Subprogram Control Example of program 1 When there are 3 subprogram calls (known as 3 nesting levels) Main program Subprogram 1 Subprogram 2 Subprogram 3 L10; L20; G22L1; G22L10; G22L20; (1)’ (2)’ (3)’ M02; G23; G23;… -
Page 303: Figure Rotation; G22 I_ J_ K
13. Program Support Functions 13.3 Subprogram Control Example of program 2 The G22 H_ ; G23 H_ ; commands designate the sequence Nos. in a program with a call instruction. G22H__ ; G23H__ ; L123; G22H3; N100___; G22L123; N200_; N300___; N3___;…
-
Page 304
13. Program Support Functions 13.3 Subprogram Control Command format G22 I__ J__ K__ L__ H__ P__ ,D__; or, G22 I__ J__ K__ <File name> H__ P__ ,D__ ; : Subprogram call command I, J, K : Rotation center : Program No. in subprogram to be called. (Own program if omitted.) Note that L can be omitted only during memory operation and MDI operation. -
Page 305
13. Program Support Functions 13.3 Subprogram Control (4) If the subprogram start point and end point are not on the same circle having the commanded figure rotation center coordinates as the center, the axis will interpolate using the subprogram’s end point as the start point, and the end point in the first movement command block in the rotated subprogram as the end point. -
Page 306: Variable Commands
13. Program Support Functions 13.4 Variable Commands 13.4 Variable Commands Function and purpose Programming can be endowed with flexibility and general-purpose capabilities by designating variables, instead of giving direct numerical values to particular addresses in a program, and by assigning the values of those variables as required when executing a program. Command format #ΔΔΔ…
-
Page 307
13. Program Support Functions 13.4 Variable Commands (2) Type of variables The following table gives the types of variables. Type of variable Function • Can be used in common Common variables Common Common variables 1 variables 2 throughout main, sub and macro programs. -
Page 308
13. Program Support Functions 13.4 Variable Commands (Note 5) When the parameter «#1052 MemVal» is set to «1» in multi-part system, a part or all of common variable «#100 to #199» and «#500 to #999» can be shared and used between part systems. -
Page 309
13. Program Support Functions 13.4 Variable Commands When multi-part system «Common variable for each part system #100 to #199» in other part system can be used. «-100» is set to #100 of 2nd part system. #200100=-100; The variable value of #102 of 2nd part system is set to #101 #101=#200102;… -
Page 310
13. Program Support Functions 13.4 Variable Commands (3) Variable quotations Variables can be used for all addresses accept L(O), N and / (slash). (a) When the variable value is used directly: X#1……… Value of #1 is used as the X value. (b) When the complement of the variable value is used: X−#2……. -
Page 311: User Macro Specifications
13. Program Support Functions 13.5 User Macro Specifications 13.5 User Macro Specifications 13.5.1 User Macro Commands; G65, G66, G66.1, G67, G68(G23) Function and purpose By combining the user macros with variable commands, it is possible to use macro program call, arithmetic operation, data input/output with PLC, control, decision, branch and many other instructions for measurement and other such applications.
-
Page 312: Macro Call Command
13. Program Support Functions 13.5 User Macro Specifications 13.5.2 Macro Call Command Function and purpose Included among the macro call commands are the simple calls which apply only to the instructed block and also modal calls (types A and B) which apply to each block in the call modal. Simple macro calls Main program Subprogram (Ll…
-
Page 313
13. Program Support Functions 13.5 User Macro Specifications Address and variable number Call instructions and usable address correspondence Argument designation I Variable in macro G65, G66 G66.1 address ∗ ∗ ∗ ∗ : Can be used. : Cannot be used. ∗… -
Page 314
13. Program Support Functions 13.5 User Macro Specifications (2) Argument designation II Format : A__ B__ C__ I__ J__ K__ I__ J__ K__• • • • Detailed description (a) In addition to address A, B and C, up to 10 groups of arguments with I, J, K serving as 1 group can be designated. -
Page 315
13. Program Support Functions 13.5 User Macro Specifications Modal call A (movement command call) Subprogram Main program To subprogram G65L l 1 Pp1 <argument>; To main program To subprogram When the block with a movement command is commanded between G66 and G67, the movement command is first executed and then the designated user macro subprogram is executed. -
Page 316
13. Program Support Functions 13.5 User Macro Specifications (Example) Drill cycle N1 G90 G54 G0 X0Y0Z0; N2 G91 G00 X-50.Y-50.Z-200.; N3 G66 L9010 R-10.Z-30.F100; L9010 N10 G00 Z #18 M0; N4 X-50.Y-50.; To subprogram after axis command execution N20 G09 G01 Z #26 F#9; N5 X-50.;… -
Page 317
13. Program Support Functions 13.5 User Macro Specifications Modal call B (for each block) The specified user macro subprogram is called unconditionally for each command block which is assigned between G66.1 and G67 and the subprogram is executed the specified number of times. Format G66.1 L__ P__ argument ;… -
Page 318
13. Program Support Functions 13.5 User Macro Specifications G code macro call User macro subprogram with prescribed program numbers can be called merely by issuing the G code command. Format G ** argument ; :G code for macro call Detailed description (1) The above instruction functions in the same way as the instructions below, and parameters are set for each G code to determine the correspondence with the instructions. -
Page 319
13. Program Support Functions 13.5 User Macro Specifications Miscellaneous command macro call (for M, S, T, B code macro call) The user macro subprogram of the specified program number can be called merely by issuing an M (or S, T, B) code. (Only entered codes apply for M but all S, T and B codes apply.) Format M** ;… -
Page 320
13. Program Support Functions 13.5 User Macro Specifications Differences between G22 and G65 commands (1) The argument can be designated for G65 but not for G22. (2) The sequence number can be designated for G22 but no for G65, G66 and G66.1. (3) G22 executes a subprogram after all the commands except M, P, H and L(O) in the G22 block have been executed, but G65 branches to the subprogram without any further operation. -
Page 321: Ascii Code Macro
13. Program Support Functions 13.5 User Macro Specifications 13.5.3 ASCII Code Macro Function and purpose A macro program can be called out by setting the correspondence of a subprogram (macro program) pre-registered with the parameters to codes, and then commanding the ASCII code in the machining program.
-
Page 322
13. Program Support Functions 13.5 User Macro Specifications Command format ∗∗∗∗; Designates the address and code ASCII code for calling out macro (one character) ∗∗∗∗ Value or expression output to variable (Setting range: ±999999.9999) Detailed description (1) The command above functions in the same way as that below. The correspondence of commands is set for each ASCII code with the parameters. -
Page 323
13. Program Support Functions 13.5 User Macro Specifications Restrictions (1) Calling a macro with an ASCII code from a program macro-called with an ASCII code A macro cannot be called with an ASCII code from a program macro-called with an ASCII code. -
Page 324
13. Program Support Functions 13.5 User Macro Specifications (4) Order of command priority If «M» is designated for the ASCII code address, the codes basically necessary for that machine will be overlapped. In this case, commands will be identified with the following priority using code values. -
Page 325: Variables
13. Program Support Functions 13.5 User Macro Specifications 13.5.4 Variables Function and purpose Both the variable specifications and user macro specifications are required for the variables which are used with the user macros. The offset amounts of the local, common and system variables among the variables for this MELDAS NC system except #33 are retained even when the unit’s power is switched off.
-
Page 326
13. Program Support Functions 13.5 User Macro Specifications Undefined variables Variables applying with the user macro specifications such as variables which have not been used even once after the power was switched on or local variables not quoted by the G65, G66 or G66.1 commands can be used as <vacant>. -
Page 327: Types Of Variables
13. Program Support Functions 13.5 User Macro Specifications 13.5.5 Types of Variables Common variables Common variables can be used commonly from any position. Number of the common variables sets depends on the specifications. Refer to «13.4 Variable commands» for details. Local variables (#1 to #33) These can be defined as an <argument>…
-
Page 328
13. Program Support Functions 13.5 User Macro Specifications [Argument specification II] Argument specification Variable in Argument specification II Variable in II address macro address macro (Note 1) Subscripts 1 to 10 for I, J, and K indicate the order of the specified command sets. They are not required to specify instructions. -
Page 329
13. Program Support Functions 13.5 User Macro Specifications (2) The local variables can be used freely in that subprogram. Main program Subprogram (1) #30=FUP [#2/#5/2] ; G65 L1 A100. B50. J10. F500; #5=#2/#30/2 ; To subprogram G22 H100 P#30 ; X#1 ;… -
Page 330
13. Program Support Functions 13.5 User Macro Specifications (3) Local variables can be used independently on each of the macro call levels (4 levels). Local variables are also provided independently for the main program (macro level 0). Arguments cannot be used for the level 0 local variables. L10 (macro level 2) Main (level 0) L1 (macro level 1) -
Page 331
13. Program Support Functions 13.5 User Macro Specifications Macro interface inputs (#1000 to #1035, #1200 to #1295) : PLC The status of the interface input signals can be ascertained by reading out the values of variable numbers #1000 to #1035, #1200 to #1295. A variable value which has been read out can be only one of 2 values: 1 or 0 (1: contact closed, 0: contact open). -
Page 332
13. Program Support Functions 13.5 User Macro Specifications System No. of Interface System No. of Interface variable points input signal variable points input signal Register R6438 bit 0 #1216 Register R6439 bit 0 #1200 #1217 Register R6439 bit 1 #1201 Register R6438 bit 1 Register R6439 bit 2 #1202… -
Page 333
13. Program Support Functions 13.5 User Macro Specifications System No. of Interface System No. of Interface variable points input signal variable points input signal #1264 Register R6442 bit 0 #1280 Register R6443 bit 0 #1265 Register R6442 bit 1 #1281 Register R6443 bit 1 #1266 Register R6442 bit 2… -
Page 334
13. Program Support Functions 13.5 User Macro Specifications System No. of Interface variable points output signal #1132 Register R6372, R6373 #1133 Register R6374, R6375 #1134 Register R6376, R6377 #1135 Register R6378, R6379 System No. of Interface System No. of Interface variable points output signal… -
Page 335
13. Program Support Functions 13.5 User Macro Specifications System No. of Interface System No. of Interface variable points output signal variable points output signal Register R6378 bit 0 #1380 Register R6379 bit 0 #1364 #1381 Register R6379 bit 1 #1365 Register R6378 bit 1 Register R6379 bit 2 #1366… -
Page 336
13. Program Support Functions 13.5 User Macro Specifications Input signal #1032 (R6436, R6437) Output signal #1132 (R6372, R6373) #1000 #1100 #1031 #1131 #1033 (R6438, R6439) #1133 (R6374, R6375) #1200 #1300 #1231 #1331 #1034 (R6440, R6441) #1134 (R6376, R6377) #1232 #1332 #1263 #1363 #1035 (R6442, R6443) -
Page 337
13. Program Support Functions 13.5 User Macro Specifications Tool compensation Tool data can be read and set using the variable numbers. Variable number range Type 1 Type 2 #10001 to #10000 + n #2001 to #2000 + n (Length dimension) #11001 to #11000 + n #2201 to #2200 + n (Length wear) -
Page 338
13. Program Support Functions 13.5 User Macro Specifications Workpiece coordinate system offset By using variable numbers #5201 to #532n, it is possible to read out the workpiece coordinate system offset data or to substitute values. (Note) The number of axes which can be controlled differs according to the specifications. The last digit of the variable No. -
Page 339
13. Program Support Functions 13.5 User Macro Specifications Alarm (#3000) The NC system can be forcibly set to the alarm state by using variable number #3000. Format #3000 = 70 (CALL#PROGRAMMER#TEL#530) : : Alarm number CALL#PROGRAMMER#TEL#530 : Alarm message Any alarm number from 1 to 9999 can be specified. The alarm message must be less than 31 characters long. -
Page 340
13. Program Support Functions 13.5 User Macro Specifications Integrating (run-out) time (#3001, #3002) The integrating (run-out) time can be read during automatic operation or automatic start or values can be substituted by using variable numbers #3001 and #3002. Contents when Variable Initialization of Type… -
Page 341
13. Program Support Functions 13.5 User Macro Specifications Feed hold, feedrate override, G09 valid/invalid By substituting the values below in variable number #3004, it is possible to make the feed hold, feedrate override and G09 functions either valid or invalid in the subsequent blocks. #3004 Bit 0 Bit 1… -
Page 342
13. Program Support Functions 13.5 User Macro Specifications G command modals Using variable numbers #4001 to #4021, it is possible to read the G modal commands which have been issued up to the block immediately before. Similarly, it is possible to read the modals in the block being executed with variable numbers #4201 to #4221. -
Page 343
13. Program Support Functions 13.5 User Macro Specifications Other modals Using variable numbers #4101 to #4120, it is possible to read the model commands assigned up to the block immediately before. Similarly, it is possible to read the modals in the block being executed with variable numbers #4301 to #4320. -
Page 344
13. Program Support Functions 13.5 User Macro Specifications Position information Using variable numbers #5001 to #5104, it is possible to read the servo deviation amounts, tool position compensation amount, skip coordinates, workpiece coordinates, machine coordinates and end point coordinates in the block immediately before. Axis No. -
Page 345
13. Program Support Functions 13.5 User Macro Specifications Basic machine coordinate system Workpiece coordinate system Read command [End point coordinates] Workpiece coordinate system [Workpiece coordinates] Machine coordinate system [Machine coordinates] (1) The positions of the end point coordinates and skip coordinates are positions in the workpiece coordinate system. -
Page 346
13. Program Support Functions 13.5 User Macro Specifications (4) The tool nose position where the tool compensation and other such factors are not considered is indicated as the end point position. The tool reference position with consideration given to tool compensation is indicated for the machine coordinates, workpiece coordinates and skip coordinates. -
Page 347
13. Program Support Functions 13.5 User Macro Specifications (Example 1) Example of workpiece position measurement An example to measure the distance from the measured reference position to the workpiece edge is shown below. Argument L9031 <Local variable> F(#9) N1 #180=#4003; X(#24)100.000 N2 #30=#5001 #31=#5002;… -
Page 348
13. Program Support Functions 13.5 User Macro Specifications Variable name setting and quotation Any name (variable name) can be given to common variables #500 to #519. It must be composed of not more than 7 alphanumerics and it must begin with a letter. Do not use «#» in variable names. It causes an alarm when the program is executed. -
Page 349
13. Program Support Functions 13.5 User Macro Specifications Number of workpiece machining times The n can be read using variables #3901 and #3902. umber of workpiece machining times By substituting a value in these variables, the number of workpiece machining times can be changed. -
Page 350
13. Program Support Functions 13.5 User Macro Specifications Tool life management (1) Definition of variable numbers (a) Designation of group No. #60000 The tool life management data group No. to be read with #60001 to #64700 is designated by substituting a value in this variable. If a group No. is not designated, the data of the group registered first is read. -
Page 351
13. Program Support Functions 13.5 User Macro Specifications (e) Data type Type M System L System Remarks Number of Number of registered registered tools tools Life current value Life current value Tool selected No. Tool selected No. Number of Number of remaining remaining registered tools registered tools… -
Page 352
13. Program Support Functions 13.5 User Macro Specifications Variable No. Item Type Details Data range 60500 Group No. Each group/ This group’s No. 1 to 99999999 +*** registration No. 61000 Tool No. Tool No. 1 to 99999999 +*** (Designate the group No. -
Page 353
13. Program Support Functions 13.5 User Macro Specifications Example of program for tool life management (1) Normal commands #101 = #60001 ; ….. Reads the number of registered tools. #102 = #60002 ; ….. Reads the life current value. #103 = #60003 ; ….. Reads the tool selection No. #60000 = 10 ;… -
Page 354
13. Program Support Functions 13.5 User Macro Specifications Precautions for tool life management (1) If the tool life management system variable is commanded without designating a group No., the data of the group registered at the head of the registered data will be read. (2) If a non-registered group No. -
Page 355
13. Program Support Functions 13.5 User Macro Specifications Reading the parameters System data can be read in with the system variables. (Note) These can be used only with some models. Variable No. Application #100000 Parameter # designation #100001 Part system No. designation #100002 Axis No./spindle No. -
Page 356
13. Program Support Functions 13.5 User Macro Specifications (4) Parameter read (#100010) The designated parameter data is read with this system variable. The following data is read according to the parameter type. Type Read data Value The values displayed on the Parameter screen are output. Text ASCII codes are converted into decimal values. -
Page 357
13. Program Support Functions 13.5 User Macro Specifications Example of parameter read macro program <Macro specifications> Q341 A_. Q_ . ; A_..Storage common variable Designates the common variable No. for storing the data read in. Q_..Parameter # designation For an axis/spindle parameter, designates the axis/spindle No. -
Page 358
13. Program Support Functions 13.5 User Macro Specifications Reading PLC data PLC data can be read in with the system variables. (Note 1) These can be used only with some models. (Note 2) The read devices are limited. Variable No. Application #100100 Device type designation… -
Page 359
13. Program Support Functions 13.5 User Macro Specifications (2) Device No. designation (#100101) The device to be read in is designated by substituting the device No. in this system variable. Convert a device expressed as a hexadecimal into a decimal when designating. If the data is read without designating this number, the data will be read in the same manner as if the minimum device No. -
Page 360
13. Program Support Functions 13.5 User Macro Specifications (4) Bit designation (#100103) (a) System variable for bit designation The bit to be read in is designated by substituting the bit designation value in this system variable. This designation is valid only when reading the bits for a 16-bit device, and is invalid in all other cases. -
Page 361
13. Program Support Functions 13.5 User Macro Specifications Examples of programs for reading PLC data (1) To read a bit device #100100 = 0 ; …. Designates [M device]. #100101 = 0 ; …. Designates [Device No. 0]. #100102 = 0 ; …. Designates [Bit]. #100 = #100110 ;… -
Page 362
13. Program Support Functions 13.5 User Macro Specifications Examples of using macro program for reading PLC data <Macro specifications> G340 F_. A_. Q_. H_. ; F_….Number of bytes designation F0..Designates bit. F1..Designates one byte. F2..Designates two bytes. A_. -
Page 363
13. Program Support Functions 13.5 User Macro Specifications Time reading variables The following operations can be carried out using the system variable extension for the user macro time. (1) By adding time information system variable #3011 and #3012, the current date (#3011) and current time (#3012) can be read and written. -
Page 364
13. Program Support Functions 13.5 User Macro Specifications Examples of using time reading variable (Example 1) To read the current date (February 14, 2001) in common variable #100 #100 = #3011 ; (20010214 is inserted in #100) (Example 2) To write current time (18 hours, 13 minutes, 6 seconds) into system variable #3012 #3012 = 181306 ;… -
Page 365: Arithmetic Commands
13. Program Support Functions 13.5 User Macro Specifications 13.5.6 Arithmetic Commands A variety of arithmetic operations can be performed between variables. Command format #i = <formula> <Formula> is a combination of constants, variables, functions and operators. Constants can be used instead of #j and #k below. Definition and #i = #j Definition, substitution…
-
Page 366
13. Program Support Functions 13.5 User Macro Specifications Sequence of arithmetic operations (1) The sequence of the arithmetic operations (1) through (3) is, respectively, the functions followed by the multiplication arithmetic followed in turn by the addition arithmetic. #101 = #111 + #112∗SIN[#113] (1) Function (2) Multiplication arithmetic (3) Addition arithmetic… -
Page 367
13. Program Support Functions 13.5 User Macro Specifications Logical sum #3=100 #3 = 01100100 (binary) (OR) #4=#3 OR 14 14 = 00001110 (binary) #4 = 01101110 = 110 Exclusive #3=100 #3 = 01100100 (binary) OR (XOR) #4=#3 XOR 14 14 = 00001110 (binary) #4 = 01101010 = 106 Logical #9=100… -
Page 368
13. Program Support Functions 13.5 User Macro Specifications (14) Arccosine #521 = ACOS [100./141.421] #521 45.000 (ACOS) #522 = ACOS [100./141.421] #522 45.000 (15) Square root #571 = SQRT [1000] #571 31.623 (SQR or #572 = SQRT [1000.] #572 31.623 #573 = SQRT [10. -
Page 369
13. Program Support Functions 13.5 User Macro Specifications Arithmetic accuracy As shown in the following table, errors will be generated when performing arithmetic operations once and these errors will accumulate by repeating the operations. Arithmetic format Average error Maximum error Type of error a = b + c −… -
Page 370: Control Commands
13. Program Support Functions 13.5 User Macro Specifications 13.5.7 Control Commands The flow of programs can be controlled by IF-GOTO- and WHILE-DO-. Branching Format IF [conditional expression] GOTO n; (n = sequence number in the program) When the condition is satisfied, control branches to «n» and when it is not satisfied, the next block is executed.
-
Page 371
13. Program Support Functions 13.5 User Macro Specifications Iteration Format WHILE [conditional expression] DOm ; (m = 1, 2, 3 ..127) END m ; While the conditional expression is established, the blocks from the following block to ENDm are repeatedly executed;… -
Page 372
13. Program Support Functions 13.5 User Macro Specifications (5) WHILE — DOm must be designated first and (6) WHILE — DOm and ENDm must correspond on a ENDm last. 1:1 (pairing) basis in the same program. WHILE ~ DO1 ; END 1 ;… -
Page 373: External Output Commands
13. Program Support Functions 13.5 User Macro Specifications 13.5.8 External Output Commands Function and purpose Besides the standard user macro commands, the following macro instructions are also available as external output commands. They are designed to output the variable values or characters via the RS-232C interface.
-
Page 374
13. Program Support Functions 13.5 User Macro Specifications Data output command : DPRNT DPRNT [ l1 # v1 [ d1 c1 ] l 2 # v2 [ d2 c2 ] • • • • • • • • • • • ] : Character string : Variable number : Significant digits above decimal point… -
Page 375: Precautions
13. Program Support Functions 13.5 User Macro Specifications 13.5.9 Precautions Precautions When the user macro commands are employed, it is possible to use the M, S, T and other NC control commands together with the arithmetic, decision, branching and other macro commands for preparing the machining programs.
-
Page 376
13. Program Support Functions 13.5 User Macro Specifications Machining program display N4, N5 and N6 are processed in parallel with the control of the executable statement of N3, N6 is an executable [In execution] N3 G00 X-100. Y-100. ; statement and so it is displayed as the next [Next command]N6 G01 X#101 Y#102 command. -
Page 377: Actual Examples Of Using User Macros
13. Program Support Functions 13.5 User Macro Specifications 13.5.10 Actual Examples of Using User Macros The following three examples will be described. (Example 1) SIN curve (Example 2) Bolt hole circle (Example 3) Grid (Example 1) SIN curve θ (SIN G65 Ll1 Aa1 Bb1 Cc1 Ff1 ;…
-
Page 378
13. Program Support Functions 13.5 User Macro Specifications (Example 2) Bolt hole circle After defining the hole data with canned cycle (G72 to G89), the macro command is issued as the hole position command. Main program a1 ; Start angle b1 ;… -
Page 379
13. Program Support Functions 13.5 User Macro Specifications G28 X0 Y0 Z0; -500. T1 M06; G90 G43 Z100.H01; G54 G00 X0 Y0; G81 Z-100.R3.F100 L0 M03; 300R G65 L9920 X-500. Y-500. A0 B8 R100.; 200R To subprogram G65 L9920 X-500. Y-500. A0 B8 R200.; To subprogram -500. -
Page 380
13. Program Support Functions 13.5 User Macro Specifications L9930 (Subprogram) L9930 #101=#24 ; → #101 Start point X coordinates : x #101 = X axis start point #102=#25 ; → #102 Start point Y coordinates : y #102 = Y direction interval →… -
Page 381: G Command Mirror Image; G50.1, G51.1 / G62
13. Program Support Functions 13.6 G Command Mirror Image 13.6 G Command Mirror Image; G50.1, G51.1 / G62 Function and purpose When cutting a shape that is symmetrical on the left and right, programming time can be shortened by machining the one side and then using the same program to machine the other side. The mirror image function is effective for this.
-
Page 382
13. Program Support Functions 13.6 G Command Mirror Image Detailed description (1) At G51.1, command the mirror image axis and the coordinate to be a center of mirror image with the absolute command or incremental command. (2) At G50.1, command the axis for which mirror image is to be turned OFF. The values of x2, y2, and z2 will be ignored. -
Page 383
13. Program Support Functions 13.6 G Command Mirror Image Precautions CAUTION Turn the mirror image ON and OFF at the mirror image center. If mirror image is canceled at a point other than the mirror center, the absolute value and machine position will deviate as shown below. -
Page 384: Corner Chamfering/Corner Rounding I
13. Program Support Functions 13.7 Corner Chamfering/Corner Rounding I 13.7 Corner Chamfering/Corner Rounding I Chamfering at any angle or corner rounding is performed automatically by adding «,C_» or «,R_» to the end of the block to be commanded first among those command blocks which shape the corner with lines only.
-
Page 385
13. Program Support Functions 13.7 Corner Chamfering/Corner Rounding I Detailed description (1) The start point of the block following the corner chamfering serves as the imaginary corner intersection point. (2) When the comma in «,C» is not present, it is handled as a C command. (3) When both the corner chamfer and corner rounding commands exist in the same block, the latter command is valid. -
Page 386: Corner Rounding » ,R
13. Program Support Functions 13.7 Corner Chamfering/Corner Rounding I 13.7.2 Corner Rounding » ,R_ » Function and purpose The imaginary corner, which would exist if the corner were not to be rounded, is rounded with the arc having the radius which is commanded by «,R_» only when configured of linear lines. Command format N100 G01 X__ Y__ , R__ ;…
-
Page 387: Linear Angle Command
13. Program Support Functions 13.8 Linear Angle Command 13.8 Linear Angle Command Function and purpose The end point coordinates are calculated automatically by commanding the linear angle and one of the end point coordinate axes. Command format N1 G01 Xx ) Aa N1 G01 Xx ) A−a…
-
Page 388: Geometric Command
13. Program Support Functions 13.9 Geometric Command 13.9 Geometric Command Function and purpose When it is difficult to find the intersection point of two straight lines with a continuous linear interpolation command, this point can be calculated automatically by programming the command for the angle of the straight lines.
-
Page 389
13. Program Support Functions 13.9 Geometric Command Detailed description (1) Automatic calculation of two-arc contact When two continuous circular arcs contact with each other and it is difficult to find the contact, the contact is automatically calculated by specifying the center coordinates position or radius of the first circular arc and the end point (absolute position) and center position or radius of the second circular arc. -
Page 390
13. Program Support Functions 13.9 Geometric Command (2) Automatic calculation of linear-arc intersection When it is difficult to find the intersections of a given line and circular arc, the intersections are automatically calculated by programming the following blocks. Example G18 G01 Aa1 Ff1 ; G02 Xxc Zzc Ii2 Kk2 Hh2 Ff2 ;… -
Page 391
13. Program Support Functions 13.9 Geometric Command (4) Automatic calculation of linear-arc contact When it is difficult to find the contact of a given line and circular arc, the contact is automatically calculated by programming the following blocks. Example G01 Aa1 Ff1 ; G03 Xxc Zzc Rr1 Ff1 ;… -
Page 392: Circle Cutting; G12, G13
13. Program Support Functions 13.10 Circle Cutting; G12, G13 13.10 Circle Cutting; G12, G13 Function and purpose Circle cutting starts the tool from the center of the circle, and cuts the inner circumference of the circle. The tool continues cutting while drawing a circle and returns to the center position. Command format G12 (G13) I__ D__ F__ ;…
-
Page 393
13. Program Support Functions 13.10 Circle Cutting; G12, G13 Example of program (Example 1) G12 I5000 D01 F100 ; (Input setting unit 0.01) When compensation amount is +10.00mm Tool Compensation 10.000m amount 50.000m Radius Precautions (1) If the offset No. «D» is not issued or if the offset No. is illegal, the program error (P170) will occur. -
Page 394: Parameter Input By Program; G10, G11.1
13. Program Support Functions 13.11 Parameter Input by Program; G10, G11.1 13.11 Parameter Input by Program; G10, G11.1 Function and purpose The parameters set from the setting and display unit can be changed in the machining programs. The data format used for the data setting is as follows. Command format G10 L70 ;…
-
Page 395: Macro Interrupt; Ion, Iof
13. Program Support Functions 13.12 Macro Interrupt; ION, IOF 13.12 Macro Interrupt; ION, IOF Function and purpose A user macro interrupt signal (UIT) is input from the machine to interrupt the program being currently executed and instead call another program and execute it. This is called the user macro interrupt function.
-
Page 396
13. Program Support Functions 13.12 Macro Interrupt; ION, IOF Outline of operation (1) When a user macro interrupt signal (UIT) is input after an ION a1 ; command is issued by the current program, interrupt program La1 is executed. When an G23; command is issued by the interrupt program, control returns to the main program. -
Page 397
13. Program Support Functions 13.12 Macro Interrupt; ION, IOF Interrupt type Interrupt types 1 and 2 can be selected by the parameter «#1113 INT_2». [Type 1] • When an interrupt signal (UIT) is input, the system immediately stops moving the tool and interrupts dwell, then permits the interrupt program to run. -
Page 398
13. Program Support Functions 13.12 Macro Interrupt; ION, IOF [Type 1] Main program block(2) block(3) block(1) If the interrupt program contains a move or miscellaneous function command, the reset block (2) is lost. block(3) block(1) block(2) Interrupt program If the interrupted program contains no move User macro interrupt and miscellaneous commands, it resumes operation from where it left in block (2), that is,… -
Page 399
13. Program Support Functions 13.12 Macro Interrupt; ION, IOF Calling method User macro interrupt is classified into the following two types depending on the way an interrupt program is called. These two types of interrupt are selected by parameter «#1229 set01/bit0». Both types of interrupt are included in calculation of the nest level. -
Page 400
13. Program Support Functions 13.12 Macro Interrupt; ION, IOF Returning from user macro interrupt G23 (H__) ; An G23 command is issued in the interrupt program to return to the main program. Address H is used to specify the sequence number of the return destination in the main program. The blocks from the one next to the interrupted block to the last one in the main program are first searched for the block with designated sequence number. -
Page 401
13. Program Support Functions 13.12 Macro Interrupt; ION, IOF Modal information variables (#4401 to #4520) Modal information when control passes to the user macro interrupt program can be known by reading system variables #4401 to #4520. The unit specified with a command applies. System variable Modal information #4401 to #4421… -
Page 402
13. Program Support Functions 13.12 Macro Interrupt; ION, IOF Parameters Refer to the Setup Manual for details on the setting methods. (1) Subprogram call validity «#1229 set 01/bit 0» 1 : Subprogram type user macro interrupt 0 : Macro type user macro interrupt (2) Status trigger mode validity «#1112 S_TRG»… -
Page 403: Tool Change Position Return; G30.1 To G30.6
13. Program Support Functions 13.13 Tool Change Position Return 13.13 Tool Change Position Return; G30.1 to G30.6 Function and purpose By specifying the tool changing position in a parameter «#8206 TOOL CHG. P» and also specifying a tool changing position return command in a machining program, the tool can be changed at the most appropriate position.
-
Page 404
13. Program Support Functions 13.13 Tool Change Position Return Example of operates (1) The figure below shows an example of how the tool operates during the tool change position return command. (Only operations of X and Y axes in G30.1 to G30.3 are figured.) G30.3 Tool changing position G30.1… -
Page 405
13. Program Support Functions 13.13 Tool Change Position Return (2) After all necessary tool changing position return is completed by a G30.n command, tool changing position return complete signal TCP (XC93) is turned on. When an axis out of those having returned to the tool changing position by a G30.n command leaves the tool changing position, the TCP signal is turned off. -
Page 406: Normal Line Control ; G40.1/G41.1/G42.1
13. Program Support Functions 13.14 Normal Line Control; G40.1/G41.1/G42.1 13.14 Normal Line Control ; G40.1/G41.1/G42.1 Function and purpose If the C axis is set as the normal line control axis, the C axis (rotation axis) turning will be controlled so that the tool constantly faces the normal line direction control in respect to the XY axis movement command during program operation.
-
Page 407
13. Program Support Functions 13.14 Normal Line Control; G40.1/G41.1/G42.1 Command format G40.1 X__ Y__ F__ ; G41.1 X__ Y__ F__ ; G42.1 X__ Y__1 F__ ; G40.1 :Normal line control cancel G41.1 :Normal line control left ON G42.1 :Normal line control right ON : X axis end point coordinates : Y axis end point coordinates : Feedrate… -
Page 408
13. Program Support Functions 13.14 Normal Line Control; G40.1/G41.1/G42.1 (3) Normal line control temporally cancel During normal line control, the turning operation for the normal line control axis is not carried out at the seam of the block that the movement amount is smaller than that set with the parameter (#1535 C_leng) and its previous block. -
Page 409
13. Program Support Functions 13.14 Normal Line Control; G40.1/G41.1/G42.1 (a) Normal line control type I Normal line control axis G41.1 G42.1 θ turning angle at block seam: θ < ε 1. -ε < 90° θ θ ε 180° 0° θ -ε… -
Page 410
13. Program Support Functions 13.14 Normal Line Control; G40.1/G41.1/G42.1 (b) Normal line control type II Normal line control axis G41.1 G42.1 θ turning angle at block seam: θ < ε 1. -ε < 90° θ ε θ 180° 0° -ε θ… -
Page 411
13. Program Support Functions 13.14 Normal Line Control; G40.1/G41.1/G42.1 (5) C axis turning speed Turning speed at block seam (select from type 1 or type 2) Item Type 1 Type 2 Normal line (a) Rapid traverse (a) Rapid traverse control axis •… -
Page 412
13. Program Support Functions 13.14 Normal Line Control; G40.1/G41.1/G42.1 Item Type 1 Type 2 Normal line (b) Cutting feed (b) Cutting feed control axis • Dry run OFF The feedrate at the tool nose is the F turning speed command. The normal line control axis The normal line control axis turning speed at block seam turning speed is the normal line control axis… -
Page 413
13. Program Support Functions 13.14 Normal Line Control; G40.1/G41.1/G42.1 Item Type 1 Type 2 Normal line The normal line control axis turning speed is The feedrate at the tool nose is the F control axis the rotation speed obtained by feedrate F. command. -
Page 414
13. Program Support Functions 13.14 Normal Line Control; G40.1/G41.1/G42.1 <Supplements> The corner arc is not inserted into the straight line that is smaller than a linear-arc, arc-arc, linear-block with no movement, block with no movement-linear or radius of the arc to be inserted. Corner R is not inserted. -
Page 415
13. Program Support Functions 13.14 Normal Line Control; G40.1/G41.1/G42.1 Precautions (1) During normal line control, the program coordinates are updated following the normal line control axis movement. Thus, program the normal line control with the program coordinate system. (2) The normal line control axis will stop at the turning start position at the single block, cutting block start interlock and block start interlock. -
Page 416
13. Program Support Functions 13.14 Normal Line Control; G40.1/G41.1/G42.1 (Continued from the previous page) Function name Notes High-accuracy control This cannot be commanded during normal line control. A program error (P29) will occur. The normal line control command during high-accuracy control cannot also be issued. A program error (P29) will occur. -
Page 417: High-Accuracy Control ; G61.1, G08
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08 13.15 High-accuracy Control ; G61.1, G08 Function and purpose This function aims to improve the error caused by the accuracy of the control system during machine machining. The parameter method and G code command method, which turn initial high-accuracy ON, are used to enter the high-accuracy control mode.
-
Page 418
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08 Command format G61.1 F__ ; G61.1 : High-accuracy control mode ON : Feedrate command The high-accuracy control mode is validated from the block containing the G61.1 command. The «G61.1» high-accuracy control mode is canceled with one of the G code group 13’s functions. — G61 (Exact stop check mode) — G62 (Automatic corner override) — G63 (Tapping mode) -
Page 419
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08 Detailed description (1) Feedrate command F is clamped with ″#2110 Clamp(H-precision)″ (Cutting feedrate during high-accuracy control mode for clamp function) set by the parameter. (2) Rapid traverse rate enables «#2109 Rapid(H-precision)» (Rapid traverse rate during high-accuracy control mode) set by the parameter. -
Page 420
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08 Pre-interpolation acceleration/deceleration Acceleration/deceleration control is carried out for the movement commands to suppress the impact when the machine starts or stops moving. However, with conventional post-interpolation acceleration/deceleration, the corners at the block seams are rounded, and path errors occur regarding the command shape. -
Page 421
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08 (2) Path control in circular interpolation commands When commanding circular interpolation with the conventional post-interpolation acceleration/ deceleration control method, the path itself that is output from the CNC to the servo runs further inside the commanded path, and the circle radius becomes smaller than that of the commanded circle. -
Page 422
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08 Optimum speed control (1) Optimum corner deceleration By calculating the angle of the seam between blocks, and carrying out acceleration/ deceleration control in which the corner is passed at the optimum speed, highly accurate edge machining can be realized. -
Page 423
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08 The accuracy coefficient differs according to parameter «#8201 COMP CHANGE». #8201 COMP CHANGE Accuracy coefficient used #8019 R COMPEN #8022 CORNER COMP The corner speed V0 can be maintained at a set speed or more so that the corner speed does not drop too far. -
Page 424
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08 (2) Arc speed clamp During circular interpolation, even when moving at a constant speed, acceleration is generated as the advance direction constantly changes. When the arc radius is large compared to the commanded speed, control is carried out at the commanded speed. However, when the arc radius is relatively small, the speed is clamped so that the generated acceleration does not exceed the tolerable acceleration/deceleration speed before interpolation, calculated with the parameters. -
Page 425
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08 (Note 3) The «R COMPEN» is valid only when the arc speed clamp is applied. To reduce the radius reduction error when not using the arc speed clamp, the commanded speed F must be lowered. -
Page 426
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08 (2) Reduction of arc radius reduction error amount using feed forward control With the high-accuracy control, the arc radius reduction error amount can be greatly reduced by combining the pre-interpolation acceleration/deceleration control method above-mentioned and the feed forward control/SHG control. -
Page 427
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08 Arc entrance/exit speed control There are cases when the speed fluctuates and the machine vibrates at the joint from the straight line to arc or from the arc to straight line. This function decelerates to the deceleration speed before entering the arc and after exiting the arc to reduce the machine vibration. -
Page 428
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08 (Example 2) When using corner deceleration <Program> <Operation> G61.1 ; • • N1 G01 X-10. F3000 ; N2 G02 X5. Y-5. I2.5 ; N3 G01 X10. ; • • <Deceleration pattern> Speed Commanded speed Arc clamp speed… -
Page 429
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08 Circular error radius compensation control for each axis When the roundness at the machine end is, compared to the reference circle, expanded at an axis creating an ellipsis state, compensation is carried out for each axis to make a perfect circle. The validity of this control can be changed with control parameter «#8108 R COMP Select». -
Page 430
13. Program Support Functions 13.15 High-accuracy Control ; G61.1, G08 Relation with other functions (1) The modals must be set as shown below when commanding G08P1. Function G code High-speed high-accuracy control II, G05 P0 High-speed machining cancel Cylindrical interpolation cancel G07.1 High-accuracy control cancel G08 P0… -
Page 431: High-Speed Machining Mode; G05, G05.1
13. Program Support Functions 13.16 High-speed Machining Mode; G05, G05.1 13.16 High-speed Machining Mode; G05, G05.1 13.16.1 High-speed Machining Mode I,II; G05 P1, G05 P2 Function and purpose This function runs a machining program for which a freely curved surface has been approximated by fine segments at high speed.
-
Page 432
13. Program Support Functions 13.16 High-speed Machining Mode; G05, G05.1 Detailed description (1) The override, maximum cutting speed clamp, single block operation, dry run, manual interruption and graphic trace and high-accuracy control mode are valid even during the high-speed machining mode I/II. (2) When using the high-speed machining mode II mode, set «BIT1″… -
Page 433
13. Program Support Functions 13.16 High-speed Machining Mode; G05, G05.1 Restrictions (1) If ″G05 P1(P2)″ is commanded when the option for high-speed machining mode I/(II) is not provided, a program error (P39) will occur. (2) The automatic operation process has the priority in the high-speed machining mode I/II , so the screen display, etc., may be slowed down. -
Page 434: High-Speed High-Accuracy Control; G05, G05.1
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1 13.17 High-speed High-accuracy Control; G05, G05.1 13.17.1 High-speed High-accuracy Control I, II Function and purpose This function runs a machining program that approximates a freely curved surface with fine segments at high speed and high accuracy. This is effective in increasing the speed of machining dies of a freely curved surface.
-
Page 435
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1 Detailed description (1) The high-speed high-accuracy control I / II can be used during computer link, tape, MDI, IC card or memory operation. (2) The override, maximum cutting speed clamp, single block operation, dry run, handle interrupt and graphic trace are valid even during the high-speed high-accuracy control I / II modal. -
Page 436
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1 (2) Acceleration clamp speed With the cutting feed clamp speed during the high-speed high-accuracy control 2 mode, when the following parameter is set to «1», the speed is clamped so that the acceleration generated by each block movement does not exceed the tolerable value. -
Page 437
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1 Precautions (1) High-speed high-accuracy control I and II are the optional functions. If «G05.1 Q1» or «G05 P10000» is commanded when the option is not provided, a program error (P39) will occur. (2) The automatic operation process has the priority in the high-speed high-accuracy control I/II modal, so the screen display, etc., may be delayed. -
Page 438
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1 Relation with other functions (1) The modal state must be as shown below when commanding G05.1 Q1 and G05 P10000. Program error (P34) will occur if the conditions are not satisfied. When commanding a SSS control, refer to ″3.16.2 SSS control″… -
Page 439
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1 High-speed high-accuracy Function G code mode Subprogram call Programmable parameter input G10 L50 Programmable compensation amount G10 L10 input High-speed high-accuracy control I G05.1 Q0 cancel High-speed high-accuracy control II G05 P0 cancel Spline control… -
Page 440: Sss Control
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1 13.17.2 SSS Control Function and purpose With conventional high-accuracy control, the angle between two blocks is compared with the corner deceleration angle to determine whether to execute corner deceleration between the blocks. This can cause the speed to suddenly change between the blocks with an angle close to the corner deceleration angle, resulting in scratches or streaks.
-
Page 441
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1 Detailed description (1) The following procedures are followed to use SSS control. (a) Turn the following parameters ON beforehand. Basic specification parameter «#1267 ext03/bit0» Machining parameter «#8090 SSS ON» (b) Command «G05 P10000 ;» (high-speed high-accuracy control II ON). →SSS control is valid until «G05 P0 ;»… -
Page 442
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1 (2) The following functions can be commanded during the SSS control mode. A program error will occur if any other function is commanded. • During G code command: Program error (P34) •… -
Page 443
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1 Parameter standard values The standard values of the parameters related to SSS control are shown below. (1) Machining parameters Item Standard value 8019 R COMP 8020 DCC ANGLE 8021 COMP CHANGE 8022 CORNER COMP 8023… -
Page 444
13. Program Support Functions 13.17 High-speed High-accuracy Control; G05, G05.1 (3) Axis specification parameters Item Standard value 2010 fwd_g Feed forward gain 2068 G0fwdg G00 feed forward gain 2096 crncsp Minimum corner deceleration speed Restrictions (1) Pre-reading is executed during SSS control, so a program error could occur before the block containing the error is executed. -
Page 445: Spline; G05.1
13. Program Support Functions 13.18 Spline; G05.1 13.18 Spline; G05.1 Function and purpose This function automatically generates a spline curve that passes through a sequence of points commanded by the fine segment machining program, and interpolates the path along this curve. This allows highly accurate machining at a high speed.
-
Page 446
13. Program Support Functions 13.18 Spline; G05.1 (3) If G05.1Q2 is commanded when not in the high-speed high-accuracy control function II mode (between G05P10000 and G05P0), the program error (P34) will occur. (4) If the machining parameter «#8025 SPLINE ON» is 0 in the high-speed high-accuracy control function II mode (between G05P10000 and G05P0) and G05.1Q2 is commanded, program error (P34) will occur. -
Page 447
13. Program Support Functions 13.18 Spline; G05.1 (Note 1) If the section to be a corner is smooth when actual machining is carried out, lower the CANCEL ANG. If a smooth section becomes a corner, increase the CANCEL ANG. (Note 2) If the CANCEL ANG. ≥ DCC. ANGLE, the axis will decelerate at all corners which angle is larger than the CANCEL ANG. -
Page 448
13. Program Support Functions 13.18 Spline; G05.1 (d) When a block markedly longer than other blocks exists in spline function If the ith block length is Li in the spline interpolation mode, and it is given as «Li > Li — 1 × 8» or «Li >… -
Page 449
13. Program Support Functions 13.18 Spline; G05.1 When the above conditions are satisfied, the spline curve will be revised so that the error between P3-P4 in Fig. 2 is within the designated value. Tolerance (chord error) Spline curve Inflection point Fine segment Fig. -
Page 450
13. Program Support Functions 13.18 Spline; G05.1 When the above conditions are satisfied, the spline curve will be revised so that the error between P2-P3 in Fig. 4 is within the designated value. Spline curve Tolerance (chord error) Fine segment Fig. -
Page 451
13. Program Support Functions 13.18 Spline; G05.1 With the spline function, the high-accuracy control function is always valid. Thus, even if the curvature changes such as in this curve, the speed will be clamped so that the tolerable value of acceleration/deceleration before interpolation, which is calculated with the parameters, is not exceeded. -
Page 452: High-Accuracy Spline Interpolation ; G61.2
13. Program Support Functions 13.19 High-accuracy Spline Interpolation ; G61.2 13.19 High-accuracy Spline Interpolation ; G61.2 Function and purpose This function automatically generates a spline curve that passes through a sequence of points commanded by the fine segment machining program, and interpolates the path along this curve. This allows highly accurate machining at a high speed.
-
Page 453
13. Program Support Functions 13.19 High-accuracy Spline Interpolation ; G61.2 Example of program G91 ; G61.2 ; ……..High-accuracy spline interpolation mode ON G01 X0.1 Z0.1 F1000 ; X0.1 Z-0.2 ; Y0.1 ; X-0.1 Z-0.05 ; X-0.1 Z-0.3 ; G64 ; ……..High-accuracy spline interpolation mode OFF (1) The spline function carries out spline interpolation when the following conditions are all satisfied. -
Page 454: Scaling; G50/G51
13. Program Support Functions 13.20 Scaling; G50/G51 13.20 Scaling; G50/G51 Function and purpose By multiplying the moving axis command values within the range specified under this command by the factor, the shape commanded by the program can be enlarged or reduced to the desired size.
-
Page 455
13. Program Support Functions 13.20 Scaling; G50/G51 Detailed description (1) Specifying the scaling axis, scaling center and its factor Commanding G51 selects the scaling mode. The G51 command only specifies the scaling axis, its center and factor, and does not move the axis. Though the scaling mode is selected by the G51 command, the axis actually valid for scaling is the axis where the scaling center has been specified. -
Page 456
13. Program Support Functions 13.20 Scaling; G50/G51 Precautions (1) Scaling is not applied to the compensation amounts of tool radius compensation, tool position compensation, tool length compensation and the like. (Compensation is calculated for the shape after scaling.) (2) Scaling is valid for only the movement command in automatic operation. It is invalid for manual movement. -
Page 457
13. Program Support Functions 13.20 Scaling; G50/G51 Example of program (Example 1) -100. -200. -150. -50. -50. Scaling center -100. D01=25.000 -150. Tool path after 1/2 scaling Program path after 1/2 scaling Tool path when scaling is not applied Program path when scaling is not applied <Program>… -
Page 458
13. Program Support Functions 13.20 Scaling; G50/G51 Relation with other functions (1) G27 reference position check command When G27 is commanded during scaling, scaling is canceled at completion of the command. (2) Reference position return command (G28, G29, G30) When the G28 or G30 reference position return command is issued during scaling, scaling is canceled at the midpoint and the axis returns to the reference position. -
Page 459: Coordinate Rotation By Program; G68.1/G69.1
13. Program Support Functions 13.21 Coordinate Rotation by Program; G68.1/G69.1 13.21 Coordinate Rotation by Program; G68.1/G69.1 Function and purpose When machining a complicated shape at a position rotated in respect to the coordinate system, the shape before rotation can be programmed on the local coordinate system, rotation angle designated with the program coordinate rotation command, and the rotated shaped machined.
-
Page 460
13. Program Support Functions 13.21 Coordinate Rotation by Program; G68.1/G69.1 Detailed description (1) Always command the rotation center coordinate (x1, y1) with an absolute value. Even if commanded with an incremental address, it will not be handled as an incremental value. The rotation angle «r»… -
Page 461
13. Program Support Functions 13.21 Coordinate Rotation by Program; G68.1/G69.1 Example of program (Program coordinate rotation by absolute command) N01 G28 X0. Y0.; Local coordinate designation N02 G54 G52 X200. Y100. ; N03 T10 ; Coordinate rotation ON N04 G68.1 X-100. Y0. R60. ; Subprogram execution N05 G22 H101 ;… -
Page 462
13. Program Support Functions 13.21 Coordinate Rotation by Program; G68.1/G69.1 Example of program (Operation of only one axis was commanded by first movement command after coordinate rotation command) Command basically two axes in the rotation plane by the absolute value immediately after the coordinate rotation command. -
Page 463
13. Program Support Functions 13.21 Coordinate Rotation by Program; G68.1/G69.1 Example of program (Local coordinate designation during program coordinate rotation) (1) When «#19003 PRG coord rot type» is «0», it is on the coordinate system after coordinates rotation that the commanded position is set as the local coordinate zero point. (2) When «#19003 PRG coord rot type»… -
Page 464
13. Program Support Functions 13.21 Coordinate Rotation by Program; G68.1/G69.1 Example of program (Coordinate system designation during program coordinate rotation) When the coordinate system setting (G92) is executed during program coordinate rotation, this program operates similarly as «Local coordinate designation during program coordinate rotation». (1) When «#19003 PRG coord rot type»… -
Page 465
13. Program Support Functions 13.21 Coordinate Rotation by Program; G68.1/G69.1 Precautions (1) Always command an absolute value for the movement command immediately after G68.1 and G69.1. (2) If manual absolute is ON and manual interrupt is issued for the coordinate rotation axis, do not use automatic operation for the following absolute value command. -
Page 466
13. Program Support Functions 13.21 Coordinate Rotation by Program; G68.1/G69.1 Relation with other functions (1) Program error (P111) will occur if the plane selection code is commanded during the coordinate rotation mode. (2) Program error (P485) will occur if pole coordinate interpolation is commanded during the coordinate rotation mode. -
Page 467: Coordinate Rotation Input By Parameter; G10
13. Program Support Functions 13.22 Coordinate Rotation Input by Parameter; G10 13.22 Coordinate Rotation Input by Parameter; G10 Function and purpose If a deviation occurs between the workpiece alignment line and machine coordinate system’s coordinate axis when the workpiece is mounted, the machine can be controlled to rotate the machining program coordinates according to the workpiece alignment line deviation.
-
Page 468
13. Program Support Functions 13.22 Coordinate Rotation Input by Parameter; G10 Command format G10 I__ J__ ; G10 K__; : Horizontal vector. Command a value corresponding to ″Coord rot plane (H)″ which is set in the parameter input screen. Command range: -999999.999999 to 999999.999999 Coordinate rotation angle is automatically calculated when commanding vector contents. -
Page 469
13. Program Support Functions 13.22 Coordinate Rotation Input by Parameter; G10 Example of program (1) To use for compensating positional deviation of pallet changer Rotation movement (15 degree) N01 G28 X0 Y0 Z0 ; N12 G90 G57 G00 X0 Y0 ; G57 workpiece N02 G22 L9000 ;… -
Page 470: 3-Dimensional Coordinate Conversion; G68.1/69.1
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 13.23 3-dimensional Coordinate Conversion; G68.1/69.1 Function and purpose With the 3-dimensional coordinate conversion function, a new coordinate system can be defined by rotating and moving in parallel the zero point in respect to the X, Y and Z axes of the currently set workpiece coordinate system.
-
Page 471
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 Command format G68.1 X__ Y__ Z__ I__ J__ K__ R__ ; G68.1 : 3-dimensional coordinate conversion mode command X,Y,Z : Rotation center coordinates Designate with the absolute position of the local coordinate system. I,J,K : Rotation center axis direction (1: Designated 0: Not designated) Note that «1»… -
Page 472
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 Example of program 1 N1 G68.1 X10.Y0. Z0. I0 J1 K0 R-30.; N2 G68.1 X0. Y10. Z0. I1 J0 K0 R45.; N3 G69.1; +Y» 45° +Z» +X» P»(0,10,0) G68.1 program coordinate system (B) P(0,0,0) Local coordinate system (workpiece coordinate system) -
Page 473
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 Coordinate system (1) By issuing the 3-dimensional coordinate conversion command, a new coordinate system (G68.1 program coordinate system) will be created on the local coordinate system. (2) The coordinate system for the 3-dimensional coordinate conversion rotation center coordinates is the local coordinate system. -
Page 474
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 G68.1 multiple commands By commanding 3-dimensional coordinate conversion during the 3-dimensional coordinate conversion modal, two or more multiple commands can be issued. (1) The 3-dimensional coordinate conversion command in the 3-dimensional coordinate conversion modal is combined with the conversion in the modal. -
Page 475
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 The conversion rows Rn and Tn (n = 1, 2) are as follow. Rn conversion row I designation J designation K designation (rotation around X axis) (rotation around Y axis) (rotation around Z axis) cosR -sinR cosR… -
Page 476
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 Precautions related to arc command If the first command after the 3-dimensional coordinate conversion command was an arc shape, and the center of the arc did not change before and after the 3-dimensional coordinate conversion, an arc is drawn. -
Page 477
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 Example of program 2 This is a sample program only to explain about the operations. (To actually proceed with the machining by using this program, the dedicated tools and the tool change functions are required.) (1) Example of machining program using arc cutting In the following program example, the arc cutting (N3 block) carried out on the top of the workpiece is also carried out on the side of the workpiece. -
Page 478
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 (2) Example of machining program using fixed cycle In the following program, the bolt hole cycle (N08 block) executed on the top of the workpiece is also carried out on the side of the workpiece. By using 3-dimensional coordinate conversion, the side can be cut with the same process (N18 block). -
Page 479
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 Relation with other functions (Relation with other G codes) Pxxx in the list indicates the program error Nos. When 3-dimensional When this command is When 3-dimensional designated during coordinate conversion is coordinate conversion Format Function… -
Page 480
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 When 3-dimensional When this command is When 3-dimensional designated during coordinate conversion coordinate conversion Format Function 3-dimensional is designated is designated coordinate conversions in this modal status in the same block Polar coordinate P923 command… -
Page 481
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 When 3-dimensional When this command is When 3-dimensional designated during coordinate conversion is coordinate conversion Format Function 3-dimensional designated in this modal is designated in the coordinate conversions status same block Tool radius P922 P923… -
Page 482
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 When 3-dimensional When this command is When 3-dimensional designated during coordinate conversion is coordinate conversion Format Function 3-dimensional designated in this modal is designated in the coordinate conversions status same block G54.1 Extended workpiece P921… -
Page 483
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 When 3-dimensional When this command is When 3-dimensional designated during coordinate conversion is coordinate conversion Format Function 3-dimensional designated in this modal is designated in the coordinate conversions status same block Fixed cycle (Balling) P922 P923… -
Page 484
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 Relation with other functions (1) Circular interpolation Circular interpolation in the 3-dimensional coordinate conversion modal functions according to the coordinate value resulted by the 3-dimensional coordinate conversion. With G17, G18 and G19 commands, circular interpolation functions normally for all the planes in which 3-dimensional coordinate conversion has been executed. -
Page 485
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 (10) Fixed cycle for drilling The fixed cycle in the 3-dimensional coordinate conversion can be executed in an oblique direction for the orthogonal coordinate system. In the same manner, synchronous tapping cycle can also be executed. -
Page 486
13. Program Support Functions 13.23 3-dimensional Coordinate Conversion; G68.1/G69.1 (16) Coordinate read variable When reading the workpiece coordinate system/skip coordinate system during the 3-dimensional coordinate system conversion modal, local coordinate system and G68.1 program coordinate system can be switched with the parameter «#1563 3Dcdrc». (17) Manual operation Manual operation in the 3-dimensional coordinate conversion modal will not execute the 3-dimensional conversion. -
Page 487: Tool Center Point Control; G43.4/G43.5
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 13.24 Tool Center Point Control; G43.4/G43.5 Function and purpose The tool center point control function controls a commanded position described in the machining program to be the tool center point in the coordinate system that rotates together with a workpiece (table coordinate system).
-
Page 488
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 <Combined type> Tool center point control OFF and Tool center point control ON tool length compensation along the tool axis ON Traces of the tool center point Z(+) Z(+) Rotation X(+) Rotation Z'(+) -
Page 489
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 Programming coordinate system The end position of each block looking from the programming coordinate system is specified in the tool center point control mode. In the program, specify the position of the tool center point. The programming coordinate system is a coordinate system used for the tool center point control, and is specified either the table coordinate system (a coordinate which rotates together with a workpiece) or the workpiece coordinate system by the parameter. -
Page 490
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 Start-up (1) Start-up without movement command (a) Tool center point control type1, type2 When the tool center point control is ON, no axis movement is performed (including movement for the compensation amount). <Tool tilt>… -
Page 491
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 (b) Tool center point control type2 The rotary axis moves toward the commanded workpiece surface vector (I,J,K) direction along the movement command issued. <Tool tilt> <Table tilt> A axis (+) G91 ;… -
Page 492
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 Cancel (1) Cancellation without movement command (a) Tool center point control type1, type2 Cancellation movement for the compensation amount is not performed regardless of absolute/incremental value command. On the other hand, the tool center point control modal will be cancelled. -
Page 493
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 (3) Cancellation with movement command (When rotary axis command is issued in the same block) (a) Tool center point control type1, type2 Cancellation movement for the compensation amount is not performed regardless of absolute/incremental value command. -
Page 494
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 (2) Tool center point control type2 (a) When executing movement command to the orthogonal coordinate axis and workpiece surface angle vector command. A axis (+) G43.5 Yy1 Zz1 (i3,j3,k3) Ii1 Jj1 Kk1 Hh ; Yy2 Ii2 Jj2 Kk2 ;… -
Page 495
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 Interpolation mode There are two modes of interpolation: single axis rotation interpolation and joint interpolation. You can select one of them by parameter. (1) Single axis rotation interpolation When transforming from a start-point angle vector «r1″… -
Page 496
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 Passing singular point When passing the singular point (singular position*), there are two kinds of movements to be followed from the singular point. When using an A-C axis tilt type machinery, there are two different movements (Fig. -
Page 497
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 (1) Passing singular point type1 Select the same direction as the start point of the tool base-side rotary axis or table workpiece-side rotary axis in the block where a singular point passing is carried out. When the rotation angle of the start point is 0°, select the wider stroke limit. -
Page 498
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 (2) Passing singular point type 2 Select the one with the smaller rotary movement amount of the tool base-side rotary axis or the table workpiece-side rotary axis on the singular point. When the tool base-side rotary axis and the table workpiece have the same rotary movement amount, select the one with the tool base-side rotary axis or the table workpiece-side rotary axis that are to be rotated in the minus-coded direction. -
Page 499
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 (3) Movement in the singular point neighborhood in each interpolation mode Inter- Type of Command from a singular point Command to pass polation Command passing to a non-singular point a singular point mode sigular point Single… -
Page 500
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 Rotary Axis Prefiltering Rotary axis prefiltering means smoothing (prefiltering) the rotary axis command (tool angle shift) process, which moves the rotary axis smoothly and produces smoother cutting surface. Tool center point moves on the tracks as programmed by the rotary axis command while the command process is smoothed with this function. -
Page 501
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 Relation with other functions (Relation with other G codes) Pxxx in the list indicates the program error Nos. The function indicated at This function is This function is Format Function the left is commanded in commanded in the modal commanded in the same… -
Page 502
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 The function indicated at This function is This function is Format Function the left is commanded in commanded in the modal commanded in the same the modal of this function indicated at the left block High-speed machining… -
Page 503
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 The function indicated at This function is This function is Format Function the left is commanded in commanded in the modal commanded in the same the modal of this function indicated at the left block G17~G19… -
Page 504
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 The function indicated at This function is This function is Format Function the left is commanded in commanded in the modal commanded in the same the modal of this function indicated at the left block G43.1/G44… -
Page 505
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 The function indicated at This function is This function is Format Function the left is commanded in commanded in the modal commanded in the same the modal of this function indicated at the left block G61.1… -
Page 506
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 Relation with other functions (1) F 1-digit feed Controls so that the tool center point moves at the commanded speed. Note that speed cannot be changed with the manual handle. (2) Buffer correction Buffer correction cannot be performed during tool center point control. -
Page 507
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 (12) Automatic operation handle interruption Do not perform the automatic operation handle interruption during the tool center point control. If performed, the tool moves off the programmed track. (13) Manual / Automatic simultaneous Manual / Automatic simultaneous cannot be executed to the axes related to the tool center point control during the tool center point control. -
Page 508
13. Program Support Functions 13.24 Tool Center Point Control; G43.4/G43.5 (25) Actual feed rate display The final combined feed rate is displayed here. (26) Manual interruption When the manual interruption is executed during the feed hold or single block stop, the movement will be the one to be observed when the manual ABS is OFF when rebooting regardless of whether an absolute/incremental value command is selected. -
Page 509: Timing-Synchronization Between Part Systems
13. Program Support Functions 13.25 Timing-synchronization between Part Systems 13.25 Timing-synchronization between Part Systems CAUTION When programming a program of the multi-part system, carefully observe the movements caused by other part systems’ programs. Function and purpose The multi-axis, multi-part system complex control NC system can simultaneously run multiple machining programs independently.
-
Page 510
13. Program Support Functions 13.25 Timing-synchronization between Part Systems Command format !L__ ; : Synchronizing No. 1 to 9999 !L1; !L1; Timing- synchro- nization Detailed description (1) If !L__ is commanded from one part system, operation of the first part system’s program will wait until !L__ is commanded from the other part system’s program. -
Page 511
13. Program Support Functions 13.25 Timing-synchronization between Part Systems (3) If there is no movement command in the same block as the timing-synchronization command, when the next block movement starts, timing-synchronization may not be secured between the part systems. To synchronize the part systems when movement starts after the timing-synchronization, issue the movement command in the same block as the synchronizing command. -
Page 512: End Point Error Check Cancellation; G69
13. Program Support Functions 13.26 End Point Error Check Cancellation; G69 13.26 End Point Error Check Cancellation; G69 Function and purpose If an illegal program is given to NC, a program error will occur. However, the error point check cancellation command G69 can be used to escape a program error only in the following conditions.
-
Page 513
13. Program Support Functions 13.26 End Point Error Check Cancellation; G69 (Ex.1) Heart cum cutting Displacement is the radius difference at the start and end points ((b — a) in the illustration below). The example program is separated into two blocks of the right and left sides. G69 G03 Ya+b Jb Ff (right side) G69 G03 Y-a-b J-a ;… -
Page 514: Coordinate Read Function; G14
13. Program Support Functions 13.27 Coordinate Read Function; G14 13.27 Coordinate Read Function; G14 Function and purpose The G14 command is used to read the end point coordinates of the immediately preceding block, the machine coordinates, the workpiece coordinates, the TLM coordinates, or the skip coordinates.
-
Page 515
13. Program Support Functions 13.27 Coordinate Read Function; G14 Example of program (1) An example of p command value and reading coordinates are given. N1 G28 X0 Y0 Z0 ; N2 G90 G00 X-200. Y-100. G53 ; M60 ; (TLM switch is turned from OFF to ON.) N4 G00 G54 X-100. -
Page 516
13. Program Support Functions 13.27 Coordinate Read Function; G14 (2) An example of reading skip coordinates are given. -150 N1 G91 G28 X0 Y0 Z0 ; N2 G90 G00 X0 Y0 ; N3 X0 Y-100. ; N4 G31 X-150. Y-50. F80 ; N5 G14 X100 Y101 P4 ;… -
Page 517: Coordinates System Setting Functions
14. Coordinates System Setting Functions 14.1 Coordinate Words and Control Axes 14. Coordinates System Setting Functions 14.1 Coordinate Words and Control Axes Function and purpose There are three controlled axis for the basic specifications, but when an additional axis is added, up to four axes can be controlled.
-
Page 518: Basic Machine, Workpiece And Local Coordinate Systems
14. Coordinates System Setting Functions 14.2 Basic Machine, Workpiece and Local Coordinate Systems 14.2 Basic Machine, Workpiece and Local Coordinate Systems Function and purpose The basic machine coordinate system is fixed in the machine and it denotes that position which is determined inherently by the machine.
-
Page 519: Machine Zero Point And 2Nd, 3Rd, 4Th Reference Positions
14. Coordinates System Setting Functions 14.3 Machine Zero Point and 2nd, 3rd, 4th Reference Positions 14.3 Machine Zero Point and 2nd, 3rd, 4th Reference Positions Function and purpose The machine zero point serves as the reference for the basic machine coordinate system. It is inherent to the machine and is determined by the reference (zero) position return.
-
Page 520: Basic Machine Coordinate System Selection; G53
14. Coordinates System Setting Functions 14.4 Basic Machine Coordinate System Selection 14.4 Basic Machine Coordinate System Selection; G53 Function and purpose The basic machine coordinate system is the coordinate system that expresses the position (tool change position, stroke end position, etc.) that is characteristic to the machine. The tool is moved to the position commanded on the basic machine coordinate system with the G53 command and the coordinate command that follows.
-
Page 521: Coordinate System Setting; G92
14. Coordinates System Setting Functions 14.5 Coordinate System Setting 14.5 Coordinate System Setting; G92 Function and purpose By commanding G92, the absolute value (workpiece) coordinate system and current position display value can be preset in the command value without moving the machine. Command format G92 X__ Y__ Z__ α…
-
Page 522: Automatic Coordinate System Setting
14. Coordinates System Setting Functions 14.6 Automatic Coordinate System Setting 14.6 Automatic Coordinate System Setting Function and purpose This function creates each coordinate system according to the parameter values input beforehand from the setting and display unit when the reference position is reached with the first manual reference position return or dog-type reference position return when the NC power is turned ON.
-
Page 523: Reference (Zero) Position Return; G28, G29
14. Coordinates System Setting Functions 14.7 Reference (Zero) Position Return 14.7 Reference (Zero) Position Return; G28, G29 Function and purpose (1) After the commanded axes have been positioned by G0, they are returned respectively at rapid traverse to the first reference (zero) position when G28 is commanded. (2) By commanding G29, the axes are first positioned independently at high speed to the G28 or G30 intermediate point and then positioned by G0 at the commanded position.
-
Page 524
14. Coordinates System Setting Functions 14.7 Reference (Zero) Position Return Detailed description (1) The G28 command is equivalent to the following: α α G00 Xx α α G00 Xx and α In this case, x are the reference position coordinates and they are set by a parameter «#2037 G53ofs»… -
Page 525
14. Coordinates System Setting Functions 14.7 Reference (Zero) Position Return Example of program (Example1) G28 Xx Reference (zero) position (#1) 1st operation after power G0Xx has been switched on 2nd and subsequent operations Intermediate point G0Xx Return start position 1st operation after power has been switched on 2nd and subsequent operations… -
Page 526
14. Coordinates System Setting Functions 14.7 Reference (Zero) Position Return (Example2) G29 Xx Present position (G0)Xx G28, G30 intermediate point (x G0 Xx (Example 3) G28 Xx ; (From point A to reference (zero) position) G30 Xx ; (From point B to 2nd reference (zero) position) G29 Xx ;… -
Page 527: 2Nd, 3Rd And 4Th Reference (Zero) Position Return; G30
14. Coordinates System Setting Functions 14.8 2nd, 3rd and 4th Reference (Zero) Position Return; G30 14.8 2nd, 3rd and 4th Reference (Zero) Position Return; G30 Function and purpose The tool can return to the second, third, or fourth reference (zero) position by specifying G30 P2 (P3 or P4).
-
Page 528
14. Coordinates System Setting Functions 14.8 2nd, 3rd and 4th Reference (Zero) Position Return; G30 Detailed description (1) The second, third, or fourth reference (zero) position return is specified by P2, P3, or P4. A command without P or with P0, P1, P5 or a greater P number is ignored, returning the tool to the second reference (zero) position. -
Page 529
14. Coordinates System Setting Functions 14.8 2nd, 3rd and 4th Reference (Zero) Position Return; G30 (6) The tool length compensation amount for the axis involved is canceled after the second, third and fourth reference (zero) position returns. (7) With second, third and fourth reference (zero) position returns in the machine lock status, control from the intermediate point to the reference (zero) position will be ignored. -
Page 530: Reference Position Check; G27
14. Coordinates System Setting Functions 14.9 Reference Position Check ; G27 14.9 Reference Position Check; G27 Function and purpose This command first positions the tool at the position assigned by the program and then, if that positioning point is the first reference position, it outputs the reference position arrival signal to the machine in the same way as with the G28 command.
-
Page 531: Workpiece Coordinate System Setting And Offset ; G54 To G59 (G54.1)
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset 14.10 Workpiece Coordinate System Setting and Offset ; G54 to G59 (G54.1) Function and purpose (1) The workpiece coordinate systems facilitate the programming on the workpiece, serving the reference position of the machining workpiece as the zero point.
-
Page 532
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset Detailed description (1) The tool radius compensation amounts for the commanded axes will not be canceled even if workpiece coordinate system is switched with any of the G54 through G59 or G54.1P1 through G54.1P96 commands (2) The G54 workpiece coordinate system is selected when the power is switched ON. -
Page 533
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset (6) The offset settings of workpiece coordinate systems can be changed any number of times. (They can also be changed by G10 L2(L20) Pp1 Xx1 Zz1.) Handling when L or P is omitted G10 L2 Pn Xx Yy Zz ;… -
Page 534
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset (7) A new workpiece coordinate system 1 is set by issuing the G92 command in the G54 (workpiece coordinate system 1) mode. At the same time, the other workpiece coordinate systems 2 through 6 (G55 to G59) will move in parallel and new workpiece coordinate systems 2 through 6 will be set. -
Page 535
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset (16) A new workpiece coordinate system P1 can be set by commanding G92 in the G54.1 P1 mode. However, the workpiece coordinate system of the other workpiece coordinate systems G54 to G59, G54.1 and P2 to P48 will move in parallel with it, and a new workpiece coordinate system will be set. -
Page 536
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset Example of program (Example 1) (1) G28 X0Y0 ; (2) G53 X-1000 Y-500 ; (3) G53 X0Y0 ; Reference (zero) position Present return position (#1) position When the first reference position coordinate is zero, the basic machine coordinate system zero point and reference (zero) position return position (#1) will coincide. -
Page 537
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset (Example 3) When workpiece coordinate system G54 has shifted (−500, −500) in example 2 (It is assumed that (3) through (10) in example 2 have been entered in subprogram 01111.) (1) G28 X0 Y0 ;… -
Page 538
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset (Example 4) When six workpieces are placed on the same coordinate system of G54 to G59, and each is to be machined with the same machining. (1) Setting of workpiece offset data Workpiece1 X = -100.000 Y = -100.000 …….. -
Page 539
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset… -
Page 540
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset (Example 5) Program example when continuously using 48 sets of added workpiece coordinate system offsets. In this example, the offsets for each workpiece are set beforehand in P1 to P48 when 48 workpieces are fixed on a table, as shown in the drawing below. -
Page 541
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset (Example 6) Program example when the added workpiece coordinate system offsets are transferred to the standard workpiece coordinate system offsets and used. In this example, the workpiece coordinate system offsets for each workpiece are set beforehand in P1 to P24 when the workpiece is fixed on a rotating table, as shown in the drawing below. -
Page 542
14. Coordinates System Setting Functions 14.10 Workpiece Coordinate System Setting and Offset L2002 (Drilling) G54 G22 H100 ; Drilling in G54 coordinate system G55 G22 H100 ; In G55 G56 G22 H100 ; In G56 G57 G22 H100 ; In G57 G58 G22 H100 ;… -
Page 543: Local Coordinate System Setting; G52
14. Coordinates System Setting Functions 14.11 Local Coordinate System Setting ; G52 14.11 Local Coordinate System Setting; G52 Function and purpose The local coordinate systems can be set independently on the G54 through G59 workpiece coordinate systems using the G52 command so that the commanded position serves as the programmed zero point.
-
Page 544
14. Coordinates System Setting Functions 14.11 Local Coordinate System Setting ; G52 (Example 1) Local coordinates for absolute value mode (The local coordinate system offset is not cumulated) 2500 (1) G28X0Y0 ; (2) G00G90X1. Y1. ; 2000 (3) G92X0Y0 ; (4) G00X500Y500 ;… -
Page 545
14. Coordinates System Setting Functions 14.11 Local Coordinate System Setting ; G52 (Example 3) When used together with workpiece coordinate system 1000 1000 Workpiece coordinate system (parameter setting value) 500 2000 (1) G28X0Y0 ; (2) G00G90G54X0Y0 ; 3000 (3) G52X500Y500 ; (4) G22L200 ;… -
Page 546
14. Coordinates System Setting Functions 14.11 Local Coordinate System Setting ; G52 (Example 4) Combination of workpiece coordinate system G54 and multiple local coordinate systems Workpiece coordinate offset (parameter setting value) (1) G28X0Y0 ; (2) G00G90G54X0Y0 ; (3) G22L300 ; (4) G52X1. -
Page 547: Workpiece Coordinate System Preset; G92.1
14. Coordinates System Setting Functions 14.12 Workpiece Coordinate System Preset; G92.1 14.12 Workpiece Coordinate System Preset; G92.1 Function and purpose (1) This function presets the workpiece coordinate system shifted with the program command during manual operation to the workpiece coordinate system offset from the machine zero point by the workpiece coordinate offset amount by the program command (G92.1).
-
Page 548
14. Coordinates System Setting Functions 14.12 Workpiece Coordinate System Preset; G92.1 Detailed description (1) Command the address of the axis to be preset. The axis will not be preset unless commanded. (2) A program error (P35) will occur if a value other than «0» is commanded. (3) This can be commanded in the following G code lists. -
Page 549
14. Coordinates System Setting Functions 14.12 Workpiece Coordinate System Preset; G92.1 (6) When movement command is issued in machine lock state Movement amount Workpiece during machine lock coordinate x after preset Workpiece coordinate Preset system coordinate value Present position Present position Workpiece coordinate y after preset… -
Page 550
14. Coordinates System Setting Functions 14.12 Workpiece Coordinate System Preset; G92.1 (8) Setting local coordinate system with G52 Local coordinates x Workpiece coordinate x after preset Present position Present position Preset Local coordinates y Local coordinate zero point Workpiece coordinate y after preset Workpiece coordinate Workpiece coordinate… -
Page 551
14. Coordinates System Setting Functions 14.12 Workpiece Coordinate System Preset; G92.1 Example of program The workpiece coordinate system shifted with G92 is preset with G92.1. 1500 1500 G92.1 command 1000 1000 preset Workpiece zero point after G92 command 1000 1000 1500 1500 Workpiece coordinate zero point… -
Page 552: Coordinate System For Rotary Axis
14. Coordinates System Setting Functions 14.13 Coordinate System for Rotary Axis 14.13 Coordinate System for Rotary Axis Function and purpose The axis designated as the rotary axis with the parameters is controlled with the rotary axis’ coordinate system. The rotary axis includes the rotating type (short-cut valid/invalid) and linear type (workpiece coordinate position linear type, all coordinate position linear type).
-
Page 553
14. Coordinates System Setting Functions 14.13 Coordinate System for Rotary Axis Example of operation Examples of differences in the operation and counter displays according to the type of rotation coordinate are given below. (The workpiece offset is set as 0°.) (1) Rotary type (short-cut invalid) (a) The machine coordinate position, workpiece coordinate position and current position are displayed in the range of 0 to 359.999°. -
Page 554
14. Coordinates System Setting Functions 14.13 Coordinate System for Rotary Axis (3) Linear type (workpiece coordinate position linear type) (a) The coordinate position counter other than the workpiece coordinate position is displayed in the range of 0 to 359.999°. The workpiece coordinate position is displayed in the range of 0 to ±99999.999°. (b) The movement is the same as the linear axis. -
Page 555: Measurement Support Functions
15. Measurement Support Functions 15.1 Automatic Tool Length Measurement; G37.1 15. Measurement Support Functions 15.1 Automatic Tool Length Measurement; G37.1 Function and purpose These functions issue the command values from the measuring start position as far as the measurement position, move the tool in the direction of the measurement position, stop the machine once the tool has arrived at the sensor, cause the NC system to calculate automatically the difference between the coordinate values at that time and the coordinate values of the commanded measurement position and provide this difference as the tool offset amount.
-
Page 556
15. Measurement Support Functions 15.1 Automatic Tool Length Measurement; G37.1 Example of execution (1) For new measurement Reference position (Z0) Tool G28 Z0; T01; M06 T02; G90 G00 G43 Z0 H01; -100 G37.1 Z-400 R200 D150 F1; Coordinate value when reached at the measurement position=-300 -200 -300-(-400)=100… -
Page 557
15. Measurement Support Functions 15.1 Automatic Tool Length Measurement; G37.1 Detailed description (1) Operation with G37.1 command Rapid traverse rate Speed Measurement allowable range D(d) D(d) F(Fp) R(r) Distance Offset amount Measuring Operation 1 position Normal completion Or no detection Stop point Alarm stop (P607) Operation 2… -
Page 558
15. Measurement Support Functions 15.1 Automatic Tool Length Measurement; G37.1 Precautions (1) Program error (P600) results if G37.1 is commanded when the automatic tool length measurement function is not provided. (2) Program error (P604) results when no axis has been commanded in the G37.1 block or when two or more axes have been commanded. -
Page 559: Skip Function; G31
15. Measurement Support Functions 15.2 Skip Function; G31 15.2 Skip Function; G31 Function and purpose When the skip signal is input externally during linear interpolation based on the G31 command, the machine feed is stopped immediately, the remaining distance is discarded and the command in the following block is executed.
-
Page 560
15. Measurement Support Functions 15.2 Skip Function; G31 Execution of G31 G90 G00 X-100000 Y0 ; G31 X-500000 F100 ; G01 Y-100000 ; G31 X0 F100 ; Y-200000 ; G31 X-50000 F100 ; Y-300000 ; X0 ; -500000 -10000 -100000 -200000 -300000 Detailed description (Readout of skip coordinates) -
Page 561
15. Measurement Support Functions 15.2 Skip Function; G31 Detailed description (G31 coasting) The amount of coasting from when the skip signal is input during the G31 command until the machine stops differs according to the parameter «#1174 skip_F» or F command in G31. The time to start deceleration to a stop after responding to the skip signal is short, so the machine can be stopped precisely with a small coasting amount δ… -
Page 562
15. Measurement Support Functions 15.2 Skip Function; G31 Detailed description (Skip coordinate readout error) (1) Skip signal input coordinate readout The coasting amount based on the position loop time constant Tp and cutting feed time constant Ts is not included in the skip signal input coordinate values. Therefore, the workpiece coordinate values applying when the skip signal is input can be read out across the error range in the following formula as the skip signal input coordinate values. -
Page 563
15. Measurement Support Functions 15.2 Skip Function; G31 Examples of compensating for coasting (1) Compensating for skip signal input coordinates #110 = Skip feedrate ; #111 = Response delay time t G31 X100. F100 ; Skip command G04 ; Machine stop check #101 = #5061 ;… -
Page 564: Multi-Step Skip Function; G31.N, G04
15. Measurement Support Functions 15.3 Multi-step Skip Function; G31.n, G04 15.3 Multi-step Skip Function; G31.n, G04 Function and purpose The setting of combinations of skip signals to be input enables skipping under various conditions. The actual skip operation is the same as with G31. The G commands which can specify skipping are G31.1, G31.2, G31.3, and G04, and the correspondence between the G commands and skip signals can be set by parameters.
-
Page 565
15. Measurement Support Functions 15.3 Multi-step Skip Function; G31.n, G04 Example of operation (1) The multi-step skip function enables the following control, thereby improving measurement accuracy and shortening the time required for measurement. Parameter settings : Skip condition Skip speed G31.1 20.0mm/min (f1) G31.2… -
Page 566: Multi-Step Skip Function 2; G31
15. Measurement Support Functions 15.4 Multi-step Skip Function 2; G31 15.4 Multi-step Skip Function 2; G31 Function and purpose During linear interpolation followed by the skip command (G31), operation can be skipped according to the conditions of the skip signal parameter Pp. Skip signal command P is specified with the external skip signal 1 to 8.
-
Page 567
15. Measurement Support Functions 15.4 Multi-step Skip Function 2; G31 Detailed description (1) The skip is specified by command speed f. Note that the F modal is not updated. (2) The skip signal is specified by skip signal parameter p. p can range from 1 to 255. If p is specified outside the range, program error (P35) occurs. -
Page 568: Speed Change Skip; G31
15. Measurement Support Functions 15.5 Speed Change Skip; G31 15.5 Speed Change Skip; G31 Function and purpose When the skip signal is detected during linear interpolation by the skip command (G31), the feedrate is changed. Command format α G31 X__ Y__ Z__ F__ F1=__ …
-
Page 569
15. Measurement Support Functions 15.5 Speed Change Skip; G31 (7) If the skip signal is input during the deceleration by the movement command completion, the speed change will be ignored. Speed Skip signal 4 Skip signal 3 Skip signal 2 (Speed change) : Invalid Skip signal 1 (Movement stop) : Valid Time Deceleration section by the movement… -
Page 570
15. Measurement Support Functions 15.5 Speed Change Skip; G31 (10) If the G31 block is started with the skip signal input, that signal is considered to rise at the same time as the block start. (11) If the skip signals for changing the speed and for stopping the movement are simultaneously input, the skip signal for stopping the movement will be valid regardless of the size of the number. -
Page 571: Programmable Current Limitation
15. Measurement Support Functions 15.6 Programmable Current Limitation 15.6 Programmable Current Limitation Function and purpose This function allows the current limit value of the servo axis to be changed to a desired value in the program, and is used for the workpiece stopper, etc. The commanded current limit value is designated with a ratio of the limit current to the rated current.
-
Page 572: Stroke Check Before Travel; G22.1/G23.1
15. Measurement Support Functions 15.7 Stroke Check Before Travel; G22.1/G23.1 15.7 Stroke Check Before Travel; G22.1/G23.1 Function and purpose By commanding the boundaries from the program with coordinate values on the machine coordinate system, machine entry into that boundary can be prohibited. This can be set only for the three basic axes.
-
Page 573
15. Measurement Support Functions 15.7 Stroke Check Before Travel; G22.1/G23.1 Precautions and restrictions (1) This function is valid only when starting the automatic operation. When interrupted with manual absolute OFF, the prohibited area will also be shifted by the interrupted amount. (2) An error will occur if the start point or end point is in the prohibited area. -
Page 574: Appendix 1. Program Error
Appendix 1. Program Error Appendix 1. Program Error (The bold characters are the message displayed in the screen.) These alarms occur during automatic operation‚ and the causes of these alarms are mainly program errors which occur‚ for instance‚ when mistakes have been made in the preparation of the machining programs or when programs which conform to the specification have not been prepared.
-
Page 575
Appendix 1. Program Error Error No. Details Remedy P 37 O, N number zero • The program Nos. are designated across a range from 1 to 99999999. A zero has been specified for program and • The sequence Nos. are designated across a sequence Nos. -
Page 576
Appendix 1. Program Error Error No. Details Remedy • Check the numerical values of the addresses P 70 Arc end point deviation large that specify the start and end points, arc • There is an error in the arc start and end center as well as the radius in the program. -
Page 577
Appendix 1. Program Error Error No. Details Remedy • Check the specifications. P 90 No spec: Thread cutting A thread cutting command was issued even though there is no thread cutting command specification. • Check the specifications. P 91 No spec: Var lead threading Variable lead thread cutting (G34) was commanded even though there is no variable lead thread cutting specification. -
Page 578
Appendix 1. Program Error Error No. Details Remedy • Check the specifications. P124 No spec: Inverse time feed There is no inverse time option. P125 G93 mode error • Reconsider the program. • A G code command that cannot be issued was issued during G93 mode. -
Page 579
Appendix 1. Program Error Error No. Details Remedy • Check the specifications. P150 No spec: Nose R compensation • Even though there were no tool radius compensation specifications, tool radius compensation commands (G41 and G42) were issued. • Even though there were no nose R compensation specifications, nose R compensation commands (G41, G42, and G46) were issued. -
Page 580
Appendix 1. Program Error Error No. Details Remedy • Add the compensation No. command to the P170 No offset number compensation command block. The compensation No. (DOO‚ TOO‚ HOO) • Check the number of compensation No. sets command was not given when the radius a correct it to a compensation No. -
Page 581
Appendix 1. Program Error Error No. Details Remedy • Command the spindle rotation speed (S) in P181 No spindle command (Tap cycle) synchronous tapping. Spindle rotation speed (S) has not been • When «#8125 Check Scode in G84» is set to commanded in synchronous tapping. -
Page 582
Appendix 1. Program Error Error No. Details Remedy • Delete the following G codes from this P201 Program error (MRC) subprogram that is called with the compound • When called with a compound type fixed type fixed cycle for turning machining I cycle for turning machining I command, the commands (G70 to G73): G27‚… -
Page 583
Appendix 1. Program Error Error No. Details Remedy • Check the number of subprogram calls and P230 Subprogram nesting over correct the program so that it does not exceed • A subprogram has been called 8 or more 8 times. times in succession from the subprogram. -
Page 584
Appendix 1. Program Error Error No. Details Remedy • Check the specifications. P270 No spec: User macro A macro specification was commanded though there are no such command specifications. • Check the specifications. P271 No spec: Macro interrupt A macro interruption command has been issued though it is not included in the specifications. -
Page 585
Appendix 1. Program Error Error No. Details Remedy • Reconsider the program and correct it so that P294 DO and END not paired the DO’s and END’s are paired off properly. The DO’s and END’s are not paired off properly. •… -
Page 586
Appendix 1. Program Error Error No. Details Remedy • Check the specifications. P381 No spec: Arc R/C Corner chamfering II /corner rounding II was specified in the arc interpolation block although corner chamfering/corner rounding II is unsupported. • Replace the block succeeding the corner P382 No corner movement chamfering/corner rounding command by… -
Page 587
Appendix 1. Program Error Error No. Details Remedy • Before commanding G111, cancel the P411 Illegal modal G111 following commands. • G111 was issued during milling mode. • Milling mode • G111 was issued during nose R • Nose R compensation compensation mode. -
Page 588
Appendix 1. Program Error Error No. Details Remedy • Check the program. P434 Compare error One of the axes did not return to the reference position when the reference position check command (G27) was executed. • An M code command cannot be issued in a P435 G27 and M commands in a block G27 command block and so the G27… -
Page 589
Appendix 1. Program Error Error No. Details Remedy P481 Illegal G code (mill) • Check the program. • An illegal G code was used during the milling mode. • An illegal G code was used during cylindrical interpolation or polar coordinate interpolation. -
Page 590
Appendix 1. Program Error Error No. Details Remedy P485 Illegal modal (mill) • Check the program. • Before issuing G12.1, issue G40 or G97. • The milling mode was turned ON during • Before issuing G12.1, issue a T command. nose R compensation or constant surface •… -
Page 591
Appendix 1. Program Error Error No. Details Remedy • Reconsider the program. P551 G06.2 knot error • Specify the knot by monotone increment. The knot (k) command value is smaller than the value for the previous block. • Match the G06.2 first block coordinate P552 Start point of 1st G06.2 err command value with the previous block end… -
Page 592
Appendix 1. Program Error Error No. Details Remedy • Check the specification. P611 No spec: Exponential function Specification for exponential interpolation is not available. • Check the program. P612 Exponential function error A movement command for exponential interpolation was issued during mirror image for facing tool posts. -
Page 593
Appendix 1. Program Error Error No. Details Remedy • Check the specifications. P930 No spec: Tool axis compen A tool length compensation along the tool axis command was issued even though there is no tool length compensation along the tool axis specification. -
Page 594: Appendix 2. Order Of G Function Command Priority
Appendix 2. Order of G Function Command Priority Appendix 2. Order of G Function Command Priority (Command in a separate block when possible) (Note) Upper level: When commanded in the same block indicates that both commands are executed simultaneously G Group G43, G44, Commanded G00 to G03…
-
Page 595
Appendix 2. Order of G Function Command Priority G Group G43, G44, Commanded G00 to G03 G17 to G19 G90, G91 G94, G95 G20, G21 G40 to G42 G code G20, G21 Possible in same block Inch/metric changeover G27 to G30 G27 to G30 are executed are executed… -
Page 596
Appendix 2. Order of G Function Command Priority G Group G50.1 Commanded G73 to G89 G98, G99 G54 to G59 G61 to G64 G66 to G67 G96, G97 G code G51.1 Group 1 G66 to G67 command is are executed During the arc executed G00 to G03.1… -
Page 597
Appendix 2. Order of G Function Command Priority G Group G50.1 Commanded G73 to G89 G98, G99 G54 to G59 G61 to G64 G66 to G67 G96, G97 G code G51.1 G20, G21 Inch/metric changeover G66 to G67 G27 to G30 are executed are executed G27 to G30… -
Page 598
Appendix 2. Order of G Function Command Priority G Group G00 to G03.1 G43, G44, Commanded G17 to G19 G90, G91 G94, G95 G20, G21 G40 to G42 G code Arc and G43, G44 cause G command error P70 G43, G44, G49 commanded last is valid. -
Page 599
Appendix 2. Order of G Function Command Priority G Group G00 to G03.1 G43, G44 Commanded G17, G19 G90, G92 G94, G95 G20, G21 G40 to G42 G code G66 to G67 are executed G66 to G67 G00 to G03.1 are executed G66 to G67 modals are… -
Page 600
Appendix 2. Order of G Function Command Priority G Group G50.1 Commanded G73 to G89 G98 to G99 G54 to G59 G61 to G65 G66 to G67 G96, G97 G code G51.1 G66 to G67 are executed G43, G44, G49 G43 to G49 Length modals are… -
Page 601
Appendix 2. Order of G Function Command Priority G Group G50.1 Commanded G73 to G89 G98, G99 G54 to G59 G61 to G67 G66 to G67 G96, G97 G code G51.1 G66 to G67 G66 to G67 G command G66 to G67 are executed are executed commanded… -
Page 603: Index
INDEX INDEX Numbers 2nd, 3rd and 4th Reference (Zero) Position Return; G30 ….515 F1-digit Feed ………………108 3-dimensional Circular Interpolation; G02.4, G03.4 ……95 Feed Functions …………….107 3-dimensional Coordinate Conversion; G68.1/69.1 ……458 Feedrate Designation and Effects on Control Axes ……116 Figure Rotation;…
-
Page 604
INDEX Normal Line Control ; G40.1/G41.1/G42.1……..394 Tape Codes………………7 NURBS Interpolation …………….100 Tape Memory Format…………….. 13 Tapping Mode; G63 …………….. 143 Thread Cutting ………………. 56 Three-dimensional Tool Radius Compensation ; G40/G41,G42..218 Optional Block Skip …………….13 Timing-synchronization between Part Systems …….. 497 Optional Block Skip ;… -
Page 605: Revision History
Revision History Date of revision Manual No. Revision details Nov. 2008 IB(NA)1500930-A First edition created.
-
Page 606
Global Service Network AMERICA EUROPE MITSUBISHI ELECTRIC AUTOMATION INC. (AMERICA FA CENTER) MITSUBISHI ELECTRIC EUROPE B.V. (EUROPE FA CENTER) Central Region Service Center GOTHAER STRASSE 10, 40880 RATINGEN, GERMANY 500 CORPORATE WOODS PARKWAY, VERNON HILLS, IL., 60061, U.S.A. TEL: +49-2102-486-0 / FAX: +49-2102-486-5910… -
Page 607
MITSUBISHI ELECTRIC ASIA PTE. LTD. (ASEAN FA CENTER) Singapore Service Center China (Shanghai) Service Center 4/F ZHI FU PLAZA, NO. 80 XIN CHANG ROAD, 307 ALEXANDRA ROAD #05-01/02 MITSUBISHI ELECTRIC BUILDING SINGAPORE 159943 SHANGHAI 200003, CHINA TEL: +65-6473-2308 / FAX: +65-6476-7439 Indonesia Service Center TEL: +86-21-2322-3030 / FAX: +86-21-2322-3000 WISMA NUSANTARA 14TH FLOOR JL. -
Page 608
Every effort has been made to keep up with software and hardware revisions in the contents described in this manual. However, please understand that in some unavoidable cases simultaneous revision is not possible. Please contact your Mitsubishi Electric dealer with any questions or comments regarding the use of this product. Duplication Prohibited This manual may not be reproduced in any form, in part or in whole, without written permission from Mitsubishi Electric Corporation.
MELDAS is a registered trademark of Mitsubishi Electric Corporation.
Other company and product names that appear in this manual are trademarks or registered trademarks of the respective companies.
Introduction
This manual is an instruction manual for NAVI LATHE for 700/70 (hereafter NAVI LATHE).
This manual explains how to operate NAVI LATHE, so read this manual thoroughly before use. Be sure to study «Precautions for Safety» on the next page and use the system safely.
Details described in this manual
CAUTION
For items described as «Restrictions» or «Usable State» in this manual, the instruction manual issued by the machine tool builder takes precedence over this manual.
Items not described in this manual must be interpreted as «not possible».
This manual is written on the assumption that all option functions are added. Confirm with the specifications issued by the machine tool builder before starting to use.
Refer to the Instruction Manual issued by each machine tool builder for details on each machine tool.
Some screens and functions may differ depending on the NC system (or its version), and some functions may not be possible. Please confirm the specifications before use.
Refer to the following documents. |
||
MITSUBISHI CNC 700/70 Series |
Instruction Manual ……………………………… |
IB-1500042 |
MITSUBISHI CNC 700/70 Series |
Setup Manual ……………………………………. |
IB-1500124 |
MITSUBISHI CNC 700/70 Series |
Programming Manual (Lathe System) |
…..IB-1500057 |
Precautions for Safety
Always read the specifications issued by the machine tool builder, this manual, related manuals and attached documents before operation or programming to ensure correct use.
Understand the NAVI LATHE, safety items and cautions before using the system.
This manual ranks the safety precautions into «DANGER», «WARNING» and «CAUTION».
DANGER |
When the user may be subject to imminent fatalities or major |
|
injuries if handling is mistaken. |
||
When the user may be subject to fatalities or major injuries if |
||
WARNING |
||
handling is mistaken. |
||
When the user may be subject to bodily injury or when property |
||
CAUTION |
||
damage may occur if handling is mistaken. |
Note that even items ranked as « CAUTION«, may lead to serious consequences depending on the situation. In any case, important information that must always be observed is described.
DANGER
Not applicable in this manual.
WARNING
1. Items related to operation
If the operation start position is set in a block which is in the middle of the program and the program is started, the program before the set block is not executed. Please confirm that G and F modal and coordinate values are appropriate. If there are coordinate system shift commands or M, S, T and B commands before the block set as the start position, carry out the required commands using the MDI, etc. If the program is run from the set block without carrying out these operations, there is a danger of interference with the machine or of machine operation at an unexpected speed, which may result in breakage of tools or machine tool or may cause damage to the operators.
Under the constant surface speed control (during G96 modal), if the axis targeted for the constant surface speed control moves toward the spindle center, the spindle rotation speed will increase and may exceed the allowable speed of the workpiece or chuck, etc. In this case, the workpiece, etc. may jump out during machining, which may result in breakage of tools or machine tool or may cause damage to the operators.
CAUTION
1. Items related to product and manual
For items described as «Restrictions» or «Usable State» in this manual, the instruction manual issued by the machine tool builder takes precedence over this manual.
Items not described in this manual must be interpreted as «not possible».
This manual is written on the assumption that all option functions are added. Confirm with the specifications issued by the machine tool builder before starting use.
Refer to the Instruction Manual issued by each machine tool builder for details on each machine tool.
Some screens and functions may differ depending on the NC system (or its version), and some functions may not be possible. Please confirm the specifications before use.
2. Items related to installation and assembly
Ground the signal cables to ensure stable system operation. Also ground the NC unit main frame, power distribution panel and machine to one point, so they all have the same potential.
3. Items related to preparation before use
Always set the stored stroke limit. Failure to set this could result in collision with the machine end.
Always turn the power OFF before connecting/disconnecting the I/O device cable. Failure to do so could damage the I/O device and NC unit.
4. Items related to screen operation
NAVI LATHE uses the following variables in order to operate the NC program.
NC program mode |
Variables used by NAVI LATHE |
User macro mode |
#150 to #197 |
MTB macro mode |
#450 to #497 |
When NC program mode is user macro mode, do not use common variables (#150 to #197). If those variables are written over, malfunction will be resulted. If mistakenly written them over, turn the NC power OFF after securing your safety. When the power is turned ON again, the system recovers the data. NC program mode is specified on the Preferences screen.
When either «TOOL REG No.» or «CYCLE» is input in each machining process screen, the cutting speed and feedrate are automatically determined using the data in the tool file screen and the cutting condition file screen. Note that the cutting speed and feedrate of each process determined once will not be changed by changing the data in the tool file screen and the cutting condition file screen.
(Continued on next page)
CAUTION
(Continued from previous page)
5. Items related to operation
Stay out of the moveable range of the machine during automatic operation. During rotation, keep hands, feet and face away from the spindle.
Carry out dry operation before actually machining, and confirm the machining program, tool offset and workpiece coordinate system offset.
If the operation start position is set from a block in the program and the program is started, the program before the set block is not executed. If there are coordinate system shift commands or M, S, T, and B commands before the block set as the starting position, carry out the required commands using the MDI, etc. There is a danger of interference with the machine if the operation is started from the set starting position block without carrying out these operations.
Program so the mirror image function is turned ON/OFF at the mirror image center. The mirror image center will deviate if the function is turned ON/OFF at a position other than the mirror image center.
6. Items related to faults and abnormalities
If the battery low warning is issued, save the machining programs, tool data and parameters in an input/output device, and then replace the battery. When the battery alarm is issued, the machining programs, tool data and parameters may be destroyed. Reload the data after replacing the battery.
If the axis overruns or emits an abnormal noise, immediately press the emergency stop button and stop the axis movement.
(Continued on next page)
CAUTION
(Continued from previous page)
7. Items related to maintenance
Incorrect connections may damage the devices, so connect the cables to the specified connectors.
Do not apply voltages other than those indicated according to specification on the connector. Doing so may lead to destruction or damage.
Do not connect or disconnect the connection cables between each unit while the power is ON.
Do not connect or disconnect the PCBs while the power is ON.
Do not connect the cable by pulling on the cable wire.
Do not short circuit, charge, overheat, incinerate or disassemble the battery.
Dispose the spent battery according to local laws.
Dispose the spent cooling fan according to local laws.
Do not replace the control unit while the power is ON.
Do not replace the operation panel I/O unit while the power is ON.
Do not replace the control section power supply PCB while the power is ON.
Do not replace the expansion PCB while the power is ON.
Do not replace the memory cassette while the power is ON.
Do not replace the cooling fan while the power is ON.
Do not replace the battery while the power is ON.
Be careful that metal cutting chips, etc., do not come into contact with the connector contacts of the memory cassette.
Do not replace the high-speed program server unit while the power is ON.
Disposal
(Note) This symbol mark is for EU countries only.
This symbol mark is according to the directive 2006/66/EC Article 20 Information for endusers and Annex II.
Your MITSUBISHI ELECTRIC product is designed and manufactured with high quality materials and components which can be recycled and/or reused.
This symbol means that batteries and accumulators, at their end-of-life, should be disposed of separately from your household waste.
If a chemical symbol is printed beneath the symbol shown above, this chemical symbol means that the battery or accumulator contains a heavy metal at a certain concentration. This will be indicated as follows:
Hg: mercury (0,0005%), Cd: cadmium (0,002%), Pb: lead (0,004%)
In the European Union there are separate collection systems for used batteries and accumulators. Please, dispose of batteries and accumulators correctly at your local community waste collection/ recycling centre.
Please, help us to conserve the environment we live in!
Contents |
||
1. OUTLINE ……………………………………………………………………………………………………… |
1 |
|
1.1 |
System Outline ……………………………………………………………………………………………… |
1 |
1.2 |
Input Procedures …………………………………………………………………………………………… |
3 |
1.3 |
Screen Configuration……………………………………………………………………………………… |
4 |
1.4 |
Starting NAVI LATHE …………………………………………………………………………………….. |
5 |
1.5 |
Setting up NAVI LATHE …………………………………………………………………………………. |
6 |
2. FUNCTIONS OF DISPLAY AREA ……………………………………………………………………. |
8 |
|
2.1 |
LIST VIEW Area ……………………………………………………………………………………………. |
9 |
2.2 OPERATION VIEW Area………………………………………………………………………………. |
11 |
|
2.3 |
Setting Area………………………………………………………………………………………………… |
12 |
2.4 |
Message Area …………………………………………………………………………………………….. |
12 |
2.5 |
Menu Display Area ………………………………………………………………………………………. |
12 |
3. BASIC OPERATIONS…………………………………………………………………………………… |
13 |
|
3.1 |
Changing Active View…………………………………………………………………………………… |
13 |
3.2 |
Changing Screen…………………………………………………………………………………………. |
13 |
3.3 |
Setting Data………………………………………………………………………………………………… |
15 |
3.4 |
Switching Windows………………………………………………………………………………………. |
18 |
3.5 |
Switching Selection Tags ……………………………………………………………………………… |
18 |
3.6 |
Inputting Operations …………………………………………………………………………………….. |
19 |
4. SCREEN SPECIFICATIONS …………………………………………………………………………. |
20 |
|
4.1 |
Starting NAVI LATHE …………………………………………………………………………………… |
20 |
4.2 |
Screen Related to the Program ……………………………………………………………………… |
21 |
4.2.1 Program Edit Screen ………………………………………………………………………. |
21 |
|
4.3 |
Screens Related to the Process Edit Functions ……………………………………………….. |
26 |
4.3.1 Process List Screen………………………………………………………………………… |
26 |
|
4.3.2 Operating Process ………………………………………………………………………….. |
27 |
|
4.3.3 Process Mode Selection Screen……………………………………………………….. |
33 |
|
4.3.4 Initial Condition Setting Screen…………………………………………………………. |
37 |
|
4.3.5 Turning Process……………………………………………………………………………… |
40 |
|
4.3.6 Copy Cut Process…………………………………………………………………………… |
46 |
|
4.3.7 Threading Screen …………………………………………………………………………… |
49 |
|
4.3.8 Grooving Screen…………………………………………………………………………….. |
53 |
|
4.3.9 Trapezoidal Grooving Screen …………………………………………………………… |
56 |
|
4.3.10 Hole Drilling Screen ………………………………………………………………………. |
59 |
|
4.3.11 EIA Screen…………………………………………………………………………………… |
61 |
|
4.3.12 Milling Hole Drilling Screen…………………………………………………………….. |
62 |
|
4.3.13 Keyway Cutting Screen …………………………………………………………………. |
75 |
|
4.3.14 Contour Cutting Screen …………………………………………………………………. |
81 |
|
4.4 |
Screens Related to File Editing ……………………………………………………………………… |
90 |
4.4.1 Tool File Screen for Turning …………………………………………………………….. |
90 |
|
4.4.2 Tool File Screen for Milling ………………………………………………………………. |
95 |
|
4.4.3 Cutting Condition File Screen for Turning…………………………………………… |
97 |
|
4.4.4 Cutting Condition File Screen for Milling…………………………………………… |
101 |
4.5 |
Screen Related to the Parameters ……………………………………………………………….. |
103 |
4.5.1 Parameter Screen…………………………………………………………………………. |
103 |
|
4.5.1.1 Parameters for Turning ………………………………………………………. |
103 |
|
4.5.1.2 Parameters for Milling ………………………………………………………… |
107 |
|
4.5.2 PREFERENCE Screen………………………………………………………………….. |
110 |
|
4.6 |
Screen Related to the Version……………………………………………………………………… |
112 |
4.6.1 Version Screen …………………………………………………………………………….. |
112 |
|
4.7 |
Program Checker Screen ……………………………………………………………………………. |
113 |
4.8 |
Guidance Function …………………………………………………………………………………….. |
122 |
4.8.1 Tool Guidance Screen …………………………………………………………………… |
123 |
|
4.8.1.1 Tool Guidance for Turning ………………………………………………….. |
123 |
|
4.8.1.2 Tool Guidance for Milling ……………………………………………………. |
125 |
|
5. PROGRAM SPECIFICATIONS…………………………………………………………………….. |
126 |
|
5.1 |
NC Program………………………………………………………………………………………………. |
127 |
5.1.1 Output Method for NC Program………………………………………………………. |
127 |
|
5.1.2 Restrictions ………………………………………………………………………………….. |
131 |
|
5.2 |
File Program ……………………………………………………………………………………………… |
133 |
5.3 |
Parameter Program ……………………………………………………………………………………. |
133 |
5.4 |
Macro Program………………………………………………………………………………………….. |
134 |
6. RESTRICTIONS FOR CNC FUNCTION SPECIFICATIONS…………………………….. |
135 |
|
7. ALARM MESSAGE…………………………………………………………………………………….. |
139 |
|
7.1 |
Error Message …………………………………………………………………………………………… |
139 |
7.2 |
Operation Message ……………………………………………………………………………………. |
142 |
APPENDIX 1. VARIABLES USED IN NAVI LATHE…………………………………………….. |
143 |
|
APPENDIX 2. PROGRAMMING EXAMPLE 1 (TURNING) ………………………………….. |
146 |
|
Appendix 2.1 Machining Drawing ………………………………………………………………………. |
146 |
|
Appendix 2.2 Process Table……………………………………………………………………………… |
147 |
|
Appendix 2.3 Condition Setting …………………………………………………………………………. |
148 |
|
Appendix 2.4 Creating Program ………………………………………………………………………… |
149 |
|
APPENDIX 3. PROGRAMMING EXAMPLE 2 (MILLING) ……………………………………. |
156 |
|
Appendix 3.1 Machining Drawing ………………………………………………………………………. |
156 |
|
Appendix 3.2 Process Table……………………………………………………………………………… |
157 |
|
Appendix 3.3 Condition Setting …………………………………………………………………………. |
158 |
|
Appendix 3.4 Creating Program ………………………………………………………………………… |
159 |
1. OUTLINE
1.1 System Outline
1. OUTLINE
1.1 System Outline
This manual is an instruction manual for NAVI LATHE for 700/70 (hereafter NAVI LATHE). The part program for the turning center is created with the NAVI LATHE.
NAVI LATHE provides the turning function and the milling function.
(1) The following machining processes can be edited.
Turning Processes
•Turning (Outer dia., inner dia., front face)
•Copy cutting (Outer dia., inner dia., front face)
•Threading (Outer dia., inner dia., front face)
•Grooving (Outer dia., inner dia., front face)
•Trapezoidal grooving (Outer dia., inner dia., front face)
•Hole drilling (Drilling, deep-hole drilling, step, tapping)
•EIA
Milling Processes
•Milling hole drilling (Drilling, deep-hole drilling, boring, tapping)
•Keyway cutting (Front face, outer surface, side surface)
•Contour cutting (Front face, outer surface, side surface)
(Note) Milling interporation specifications are required to edit the milling processes.
(2)The tool file and the cutting condition file are provided and the cutting conditions for each process are determined automatically.
(3)The operation screen consists of the LIST VIEW area and the OPERATION VIEW area. In the LIST VIEW area, the whole part program can be always viewed. In the OPERATION VIEW area, there are the guide drawings related to the input items, and the data can be easily input by using these guide drawings.
[LIST VIEW area]
The object of the NAVI LATHE is selected.
[OPERATION VIEW area] The screen is displayed
corresponding to the object selected in the LIST VIEW.
[Cutting conditions automatically determined]
Upon tool registration No. entry, the cutting conditions for each process are automatically determined based on the tool file and cutting condition file.
[Help]
[Guide drawing]
[Menu keys]
— 1 —
1. OUTLINE
1.1 System Outline
(4)Program Checker enables the machining shape of a part program to be graphically traced. With this function, errors in input data can be detected at an earlier stage.
(5)Guidance function provides an operator with error recovery information.
(6)Part program is a macro-program-based NC program. Commands can be added between processes from the edit screen of the standard MITSUBISHI CNC 700/70 Series.
(7)The macro program mentioned above can be customized by the machine tool builder.
— 2 —
1. OUTLINE
1.2 Input Procedures
1.2 Input Procedures
The input procedure for the NAVI LATHE is shown below.
The part is operated on the NAVI LATHE’s screen.
Start
File edition
Tool file
Cutting condition file
Parameter setting
Parameter file
(The parameter setting is valid even if the parameter is set after editing the NC program)
NC program selection
Newly create
Read out
Process editing:
Initial conditions Process mode selection Process data input
Turning / Copy cutting / Threading / Grooving / Trapezoidal grooving / Hole drilling / EIA / Milling hole drilling /
Keyway cutting / Contour cutting
Program check (Note) Set the tool
compensation amount and workpiece coordinate system offset to perform Program Check. This function is realized by using the 700/70 Series graphic check function.
NC program operation
Supplements
Tool file |
Cut condition file |
|
(Tool registration No. 101-) |
(Work registration No.1 to |
|
99 |
8 |
|
Tool leng. offset |
Material |
|
1 |
1 |
|
Tool leng. offset No. |
Tool applicable |
|
Tool leng. offset |
Material |
|
No. |
: rotation rate |
|
Tool diam. ffset |
||
No. |
No. |
Tool applicable |
Tool diam. offset |
: |
|
rotation rate |
||
Spindle rotation |
: |
|
No. |
||
direction |
||
Spindle rotation |
||
direction |
||
: |
Parameter setting
•M0 output
•Maximum number of spindle rotations
•Clearance
•Tool return position
•Common parameters for threading process
•Common parameters for grooving process
•Common parameters for hole drilling process
Process editing
END
— 3 —
1. OUTLINE
1.3 Screen Configuration
1.3 Screen Configuration
The screen configuration for the NAVI LATHE is shown below.
Program editing screen
Turning |
||||||||
screen |
||||||||
Process list |
||||||||
screen |
||||||||
Copy- |
||||||||
cutting |
||||||||
Initial |
screen |
|||||||
condition |
||||||||
setting screen |
Threading |
|||||||
screen |
||||||||
Process mode |
Grooving |
|||||||
selection |
||||||||
screen |
||||||||
screen |
||||||||
(For a new process, |
Trapezoidal |
|||||||
grooving |
||||||||
select a process from |
||||||||
the process mode.) |
screen |
|||||||
Hole drilling |
||||||||
screen |
||||||||
EIA screen |
||||||||
Milling |
||||||||
hole drilling |
||||||||
screen |
||||||||
Keyway |
||||||||
cutting |
||||||||
screen |
||||||||
Program |
Contour |
|||||||
cutting |
||||||||
checker |
||||||||
screen |
||||||||
Tool file |
||||||||
screen |
||||||||
Cutting |
||||||||
condition |
||||||||
file screen |
Process pattern screen
Process pattern screen
Process pattern screen
Parameter |
Preference |
|||||||||
Parameter |
||||||||||
screen |
screen |
|||||||||
Version |
||||||||||
Version |
||||||||||
screen |
||||||||||
— 4 —
1. OUTLINE
1.3 Screen Configuration |
|||||||||||
Screen name |
Details |
||||||||||
Program editing screen |
NC program is newly created and read out, etc. |
||||||||||
Process list screen |
Tool information and cutting conditions for each process of a |
||||||||||
NC program are listed. |
|||||||||||
Process mode selection |
The process mode (turning process, etc.) is selected. |
||||||||||
screen |
|||||||||||
Initial |
conditions |
setting |
The initial conditions for a NC program are set. |
||||||||
screen |
|||||||||||
Turning screen |
Various parameters for turning process are input. |
||||||||||
Turning pattern screen |
The machining patterns for turning process are input. |
||||||||||
Copy cutting screen |
Various parameters for copy cutting process are input. |
||||||||||
Copy |
cutting |
pattern |
Machining patterns for copy cutting process are input. |
||||||||
screen |
|||||||||||
Threading screen |
Various parameters for threading process are input. |
||||||||||
Grooving screen |
Various parameters for grooving process are input. |
||||||||||
Trapezoidal |
grooving |
Various parameters for trapezoidal grooving process are |
|||||||||
screen |
input. |
||||||||||
Hole drilling screen |
Various parameters for hole drilling process are input. |
||||||||||
EIA screen |
The EIA process is input. |
||||||||||
Milling |
hole |
drilling |
Various parameters for milling hole drilling process are input. |
||||||||
screen |
|||||||||||
Milling |
hole |
drilling |
The machining patterns for milling hole drilling process are |
||||||||
pattern screen |
input. |
||||||||||
Keyway cutting screen |
Various parameters for keyway cutting process are input. |
||||||||||
Contour cutting screen |
Various parameters for contour cutting process are input. |
||||||||||
Contour |
cutting |
pattern |
The machining patterns for contour cutting process are input. |
||||||||
screen |
|||||||||||
Tool file screen |
The tool data by each tool is registered. |
||||||||||
Cutting |
condition file |
The cutting conditions (cutting speed, feedrate) by each |
|||||||||
screen |
process are input, corresponding to tip material. Also, the |
||||||||||
cutting conditions (speed rate) by each process are input, |
|||||||||||
corresponding to workpiece material. |
|||||||||||
Parameter screen |
The parameters for a NC program are set. |
||||||||||
Preference screen |
The system is set up. |
||||||||||
Version screen |
The version data of the NAVI LATHE is displayed. |
||||||||||
Program checker |
The machining shape of a NC program is graphically |
||||||||||
displayed. |
|||||||||||
1.4 Starting NAVI LATHE |
|||||||||||
Select |
function, then the lathe menu to display NAVI LATHE screen. |
||||||||||
EDIT |
Program edit screen is displayed once when the power is turned ON. Then, whatever the screen previously selected with NAVI LATHE is displayed thereafter.
— 5 —
1. OUTLINE
1.5 Setting up NAVI LATHE
1.5 Setting up NAVI LATHE
Part program output from NAVI LATHE is a macro-program-based NC program. Thus, macro programs have to be registered in the NC system in advance. Also, the destinations where NC programs or NAVI LATHE’s reference files are saved, as well as the unit for data input, have to be specified prior to NAVI LATHE operations.
NAVI LATHE setup items
Item |
Details |
Standard value |
PATH |
Path to the folder in which NC program is saved. |
MEM:/ |
PROGRAM |
||
PATH |
Path to the folder in which tool file, cutting condition file |
In 700 Series: |
PARAMETER |
and parameter file are saved. |
D:/NCFILE/NAVI |
In 70 Series: |
||
MEM:/ |
||
MACRO |
Macro program mode |
1 (User Macro) |
1: User macro mode |
||
2: MTB macro mode |
||
UNIT |
Unit for data input |
2 (mm) |
1: inch |
||
2: mm |
— 6 —
1. OUTLINE
1.5 Setting up NAVI LATHE
NAVI LATHE setup procedures
(1)Open PARAMETER screen.
(2)Set «999 MAINTE» to 1.
(3)Press [PREFERENCE] menu.
(4)Select the macro type. (1:Uer macro 2:MTB macro)
(5)Press [MACRO ENTRY] menu.
(6)Press [Y] key.
(7)Enter the program path.
(8)Enter the parameter path.
(9)Select the unit. (1:inch, 2:mm)
(Addendum)
[PREFERENCE] menu is displayed.
PREFERENCE screen is displayed.
«OK?(Y/N)» message is displayed.
Macro program is registered in NC system.
When the unit is changed, turn the power OFF and ON again.
•Always carry out a macro program registration when setting up NAVI LATHE or switching «MACRO» types.
•Change «PROGRAM PATH» and «PARAMETER PATH» when necessary.
•When «UNIT» is changed, turn the power OFF and ON again.
•If the tool file, cutting condition file and parameter file do not exist in «PARAMETER PATH» folder when the power is turned ON, the system creates them.
— 7 —
2.FUNCTIONS OF DISPLAY AREA
2.FUNCTIONS OF DISPLAY AREA
The screen of the NAVI LATHE is divided into the following five areas.
(1)LIST VIEW area (Refer to «2.1 LIST VIEW Area»)
(2)OPERATION VIEW area (Refer to «2.2 OPERATION VIEW Area»)
(3)Setting area (Refer to «2.3 Setting Area»)
(4)Message area (Refer to «2.4 Message Area»)
(5)Menu display area (Refer to «2.5 Menu Display Area»)
(1) LIST VIEW area |
(2) OPERATION VIEW area |
(4) Message area
(5) Menu display area |
(3) Setting area |
<Screen example>
— 8 —
2. FUNCTIONS OF DISPLAY AREA
2.1 LIST VIEW Area
2.1 LIST VIEW Area
The object of the NAVI LATHE is selected in this area.
(1) Area bar
(2) Object
(3) Cursor
(1) Area bar
When the LIST VIEW area is active, the area bar is highlighted.
(2) Objects
The list of objects that can be selected are displayed. The object is composed of the main object and the sub object, which is a specification of the main object. The details of each object are as follows.
Main object |
Sub object |
Details |
PROGRAM |
— |
Newly creates, reads out, and deletes, etc. the NC program. |
PROCESS |
0 INIT |
Displays the currently edited process list. |
1 DR |
The settings of the selected process can be displayed and |
|
: |
changed. |
|
FILE |
TOOL |
Displays and changes the tool file. |
M TOOL |
Displays and changes the tool file for the milling machining. |
|
(Note) This is valid when the milling interporation |
||
specifications are provided. |
||
CUT CONDTN |
Displays and changes the cutting conditions for each |
|
process per tip material or workpiece material. |
||
M CUT |
Displays and changes the cutting conditions for each |
|
CONDTN |
process per tip material or workpiece material for the milling |
|
machining. |
||
(Note) This file is valid when the milling interporation |
||
specifications are provided. |
||
PARAMETER |
— |
Displays the tool option and the miscellaneous parameter to |
be used in each process. Those can be changed. |
||
VERSION |
— |
Displays the version data of the NAVI LATHE. |
(Note) If too many processes are registered and all the objects cannot be displayed, a scroll bar will be displayed. In this case, change display of the list by pressing cursor key or page key down, or by clicking on the scroll bar.
— 9 —
2. FUNCTIONS OF DISPLAY AREA
2.1 LIST VIEW Area
(3) Cursors
When the LIST VIEW area is active and the object is selected with the cursor, the display in the OPERATION VIEW area and the menu display area will be changed.
<Cursor movement>
The cursor is moved using the cursor keys or a pointing device.
Key type |
Operation of cursor |
[↑] Cursor key |
Moves the cursor one field up regardless of the main object or sub object. |
Note that if the ↑ cursor is pressed when the cursor is at the top, the cursor |
|
does not move. |
|
[↓] Cursor key |
Moves the cursor one field down regardless of the main object or sub object. |
Note that if the ↓ cursor is pressed when the cursor is at the bottom, the |
|
cursor does not move. |
|
[←] Cursor key |
When the cursor is at the sub object, moves the cursor to the previous main |
object. |
|
[→] Cursor key |
When the cursor is at the sub object, moves the cursor to the next main |
object. |
|
[Page Up] key |
Moves the displayed data toward the top. |
[Page Down] |
Moves the displayed data toward the bottom. |
key |
|
Pointing device |
Cursor jumps to the spot where clicked with a pointing device. If an object not |
selectable is clicked, cursor does not jump. |
— 10 —
2. FUNCTIONS OF DISPLAY AREA
2.2 OPERATION VIEW Area
2.2 OPERATION VIEW Area
The various data are displayed in this area. Selecting the object in the LIST VIEW area changes the contents displayed in the OPERATION VIEW area.
(1) Area bar
(2) Help
(3) Guide drawing
(4) Sub cursor
(1) Area bar
When the OPERATION VIEW area is active, the area bar is highlighted. The name of the currently edited program is displayed.
(2) Help
Quick reference on the setting items is displayed.
(3) Guide drawing
When the process is edited, a guide drawing according to the currently edited machining mode is displayed.
(4) Sub cursor
Key type |
Operation of cursor |
[↑] Cursor key |
Moves the cursor one field up. |
Note that if the ↑ cursor is pressed when the cursor is at the top, the cursor |
|
does not move. |
|
[↓] Cursor key |
Moves the cursor one field down. |
Note that if the ↓ cursor is pressed when the cursor is at the bottom, the |
|
cursor does not move. |
|
[Page Up] key |
Moves the displayed data toward the top. |
[Page Down] |
Moves the displayed data toward the bottom. |
key |
|
— 11 —
2. FUNCTIONS OF DISPLAY AREA
2.3 Setting Area
2.3 Setting Area
The value to be set to data is input.
2.4 Message Area
An error message or operation message, etc. during operation is displayed.
2.5 Menu Display Area
The screen operation is selected, and the screen is changed.
The different menus are displayed in each screen. (Refer to the chapter 4.)
— 12 —
3. BASIC OPERATIONS
3.1 Changing Active View
3. BASIC OPERATIONS
3.1 Changing Active View
To operate NAVI LATHE, activate either LIST VIEW area or OPERATION VIEW area. When the VIEW is active, the area bar is highlighted and data can be input. Use menu keys [←] and [→] or a pointing device to switch either one of the VIEWs to be activated.
3.2 Changing Screen
When the object is selected in the LIST VIEW area, the screen (contents in the OPERATION VIEW area) changes. (Refer to the section 2.1 LIST VIEW Area.)
Note that the screen cannot be changed while the OPERATION VIEW area is active.
In such a case, press the [←] menu key or click «LIST VIEW» with a pointing device to turn the LIST VIEW area active.
Operation example
(1)Open the program edit screen.
The OPERATION VIEW area is active.
(2)Press the [←] menu key.
The LIST VIEW area will turn active.
— 13 —
3.BASIC OPERATIONS
(3)Select the object with the cursor key.
(4)Press the [MODIFY] menu key.
3.2 Changing Screen
The OPERATION VIEW area will change into the screen corresponding to the selected object.
The OPERATION VIEW area will turn active.
— 14 —
3. BASIC OPERATIONS
3.3 Setting Data
3.3 Setting Data
After moving the sub cursor, input the data into the setting area and then press the [INPUT] key, and the data will be set. (The sub cursor is displayed only when the OPERATION VIEW area is active.)
Sub cursor
Setting area
— 15 —
3. BASIC OPERATIONS
3.3 Setting Data
Operation method
An example for setting the data on the hole drilling screen is shown below.
(1) Screen selection
Select the object to be changed from the LIST VIEW and press [MODIFY] menu key.
The OPERATION VIEW area will turn active.
(Refer to the section 3.2 «Changing screen».)
(2) Setting item selection |
||
Move the sub cursor with cursor keys. |
This is an example of the sub cursor |
|
movement on the hole drilling screen. |
||
(3) Data key input
Set data with the numeral keys or alphabet keys, etc.
[1] [8] [.] [0] [0] [0]
(4) [INPUT] key input
Press the [INPUT] key.
The data is set in the data setting area.
18 000
Data for the selected setting item is set. The sub cursor moves to the next position.
(Note 1) The contents in the data setting area are only displayed when [INPUT] key is not pressed and will be invalidated if the screen is changed at this time. Data for the currently selected setting item will be set when [INPUT] key is pressed.
(Note 2) If illegal data is set, an error occurs when [INPUT] is pressed. Set the correct data again.
— 16 —
3. BASIC OPERATIONS
3.3 Setting Data
Operations in the data setting area
The key is input at the position where the cursor is displayed. If a cursor is not displayed, the key input is invalid.
When a key is input, the data appears at the cursor position, and the cursor moves one character space to the right.
[→] / [←] keys: Moves the cursor one character to the left or right.
(1)The cursor is at the position shown on
the right. |
1 2 3 7 7 7 | 4 5 6 |
||||
(2) |
Press the [→] key. |
The cursor moves one character space to |
|||
the right. |
|||||
1 2 3 7 7 7 4 | 5 6 |
|||||
[DETETE] key: Deletes the character in front of the cursor.
(1) |
Move the cursor to the position where |
The cursor in the data setting area moves. |
|||
the data is to be deleted. |
1 2 3 |
4 | 5 6 |
|||
(2) |
The character in front of the cursor is |
||||
Press the [DETETE] key. |
|||||
deleted. |
|||||
1 2 3 |
| 5 6 |
||||
— 17 —
3. BASIC OPERATIONS
3.4 Switching Windows
3.4 Switching Windows
When a shortcut button on the keyboard is pressed, its corresponding window is displayed.
Button |
Application |
|||||
Displays the tool guidance window. |
||||||
LIST
?Displays the message guidance window.
Displays the checker window.
3.5 Switching Selection Tags
Menu tag
When a tag button on the keyboard is pressed, the main window and checker window can be switched over.
Button |
Application |
||||
Selects the tag on the left. |
|||||
Selects the tag on the right. |
|||||
(Note 1) Depending on the keyboard specifications, tag button may not be available.
— 18 —
3. BASIC OPERATIONS
3.6 Inputting Operations
3.6 Inputting Operations
In addition to the method of directly inputting numeric data for specific data settings, a method to input the operation results using four rules operators and function symbols can be used.
Input method
Numeric values, function symbols, operators and parentheses ( ) are combined and set in the data setting area.
The operation results appear when the [INPUT] key is pressed. Data for the currently selected setting item will be set when [INPUT] key is pressed again.
The contents in the data setting area are erased.
Examples of operator settings, |
Function symbols, setting examples |
|||||||
and results |
and results |
|||||||
Operation |
Setting |
Operation |
Function |
Function |
Setting |
Operation |
||
example |
results |
symbol |
example |
results |
||||
Addition |
=100+50 |
150.000 |
Absolute |
ABS |
=ABS |
10.000 |
||
value |
(50−60) |
|||||||
Subtraction |
=100−50 |
50.000 |
Square root |
SQRT |
=SQRT |
(3) |
1.732 |
|
Multiplication |
=12.3 4 |
49.200 |
Sine |
SIN |
=SIN |
(30) |
0.5 |
|
Division |
=100/3 |
33.333 |
Cosine |
COS |
=COS |
(15) |
0.966 |
|
Function |
=1.2 |
5.400 |
Tangent |
TAN |
=TAN |
(45) |
1 |
|
(2.5+SQRT(4)) |
Arc tangent |
ATAN |
=ATAN |
(1.3) |
52.431 |
|||
Circle ratio |
PAI |
=PAI*10 |
31.415 |
|||||
Inch |
INCH |
=INCH/10 |
2.54 |
Operation examples
(1)Set as shown below, and press the [INPUT] key.
=12 20 [INPUT]
(2)Press the [INPUT] key again.
The operation results appear in the data setting area.
240 |
Data for the selected setting item is set. The cursor moves to the next position.
Notes for using operators and functions
Division: |
Zero division causes an error. |
Square root: |
If the value in the parentheses is negative, an error occurs. |
Triangle function: |
The unit of angle θ is degree (°). |
Arc tangent: |
−90 < operation results < 90. |
Restrictions
•Always use «=» for the first character.
•Do not use the following characters as the second character or last character. Invalid as second character: , /, )
Invalid as last character: , /, (, +, —
•Make sure that the left parentheses and right parentheses are balanced.
•The 360° limit does not apply on the angle. SIN (500) is interpreted as SIN (140).
—19 —
4. SCREEN SPECIFICATIONS
4.1 Starting NAVI LATHE
4. SCREEN SPECIFICATIONS
4.1 Starting NAVI LATHE
When NAVI LATHE is started, the program edit screen will be displayed.
Screen layout
At the initial start up of NAVI LATHE, the cursor is displayed at the position of [PROGRAM] in the LIST VIEW area, and the program edit screen is displayed in the OPERATION VIEW area.
The LIST VIEW area is active.
The process program is not selected.
— 20 —
4. SCREEN SPECIFICATIONS
4.2 Screen Related to the Program
4.2 Screen Related to the Program
4.2.1 Program Edit Screen
The NC program is newly created and read out, etc. on this screen. When [PROGRAM] is selected in the LIST VIEW area, this screen is displayed.
Screen layout
The process list of the currently selected program is displayed in the LIST VIEW area.
— 21 —
4. SCREEN SPECIFICATIONS
4.2 Screen Related to the Program |
|||||
<Turning process displays> |
|||||
Process name |
Display |
Remarks |
|||
character |
|||||
Turning |
OD OPEN |
TURN-OUT ? |
A symbol that indicates the machining type |
||
(rough/finishing) is put at ?. |
|||||
OD CLOSE |
TURN-OUT ? |
||||
• Rough machining: R |
|||||
• Finishing machining: F |
|||||
ID OPEN |
TURN-IN ? |
||||
ID CLOSE |
TURN-IN ? |
||||
FACE OPEN |
TURN-FACE ? |
||||
FACE CLOSE |
TURN-FACE ? |
||||
Copy cutting |
Outer diameter |
COPY OUT ? |
A symbol that indicates the machining type |
||
(rough/finishing) is put at ?. |
|||||
Inner diameter |
COPY-IN ? |
||||
• Rough machining: R |
|||||
• Finishing machining: F |
|||||
Thread |
Outer diameter |
THD-OUT ? |
A symbol that indicates the machining type |
||
(rough/finishing) is put at ?. |
|||||
Inner diameter |
THD-IN ? |
||||
• Rough machining: R |
|||||
Face |
THD-FACE ? |
||||
• Finishing machining: F |
|||||
Groove |
Outer diameter |
GRV-OUT |
|||
Inner diameter |
GRV-IN |
||||
Face |
GRV-FACE |
||||
Trapezoidal |
Outer diameter |
TGRV-OUT ? |
A symbol that indicates the machining type |
||
grooving |
Inner diameter |
TGRV-IN ? |
(rough/finishing) is put at ?. |
||
• Rough machining: R |
|||||
Face |
TGRV-FACE ? |
||||
• Finishing machining: F |
|||||
Hole drilling |
Drill |
DR |
|||
Deep hole |
PECK |
||||
Step |
STEP |
||||
Tapping |
TAP |
||||
EIA |
EIA |
— 22 —
4. SCREEN SPECIFICATIONS
4.2 Screen Related to the Program |
||||||||||
<Milling process displays> |
||||||||||
Process name |
Display |
Remarks |
||||||||
character |
||||||||||
Milling |
Drilling |
M DR-**** |
Symbols that indicate the machining area |
|||||||
hole |
(front face/outer surface/side surface) are put at |
|||||||||
drilling |
****. |
|||||||||
Deep hole |
M PECK-**** |
Front face: FACE |
||||||||
drilling |
Outer surface: OUT |
|||||||||
Side surface: SIDE |
||||||||||
Step |
M STEP-**** |
|||||||||
Tapping |
M TAP-**** |
|||||||||
Keyway |
Front face |
K WAY-FACE ? |
A symbol that indicates machining type |
|||||||
cutting |
(rough/finishing) is put at ?. |
|||||||||
Rough machining: R |
||||||||||
Outer surface |
K WAY-OUT ? |
|||||||||
Side surface |
K WAY-SIDE ? |
Finishing machining: F |
||||||||
Contour |
Front face |
CONT-FACE ? |
||||||||
cutting |
||||||||||
Outer surface |
CONT-OUT ? |
|||||||||
Side surface |
CONT-SIDE ? |
|||||||||
Screen display item |
||||||||||
No. |
Display item |
Details |
Setting range |
|||||||
1 |
PROGRAM LIST |
Displays the program number and comment of the |
— |
|||||||
NC program that can be currently read out. |
||||||||||
— 23 —
4. SCREEN SPECIFICATIONS
4.2 Screen Related to the Program
Menus
No. |
Menu |
Details |
||
1 |
← |
Turns the LIST VIEW area active. |
||
2 |
NEW |
Newly creates the NC program. (Note 1) |
||
< Display in the setting area when pressing the menu > |
||||
O( |
) COMMENT( |
) |
||
3 |
OPEN |
Reads out the existing NC program. (Note 1) (Note 2) |
||
< Display in the setting area when pressing the menu > |
||||
O( |
) |
|||
When this menu is pressed, the cursor appears at the program list’s |
||||
name section. When the setting area is empty, select a program with |
||||
the cursor and press the [INPUT] key to read the program. |
||||
Cursor |
||||
4 |
COPY |
Copies the existing NC program to another program. (Note 1) |
||
< Display in the setting area when pressing the menu > |
||||
O( |
) → O( |
) |
||
5 |
COMMENT |
Edits the comment in the NC program. (Note 1) |
||
< Display in the setting area when pressing the menu > |
||||
O( |
) COMMENT( |
) |
||
6 |
RENAME |
Renames the existing NC program. (Note 1) |
||
< Display in the setting area when pressing the menu > |
||||
O( |
) → O( |
) |
||
7 |
DELETE |
Deletes the NC program. |
||
< Display in the setting area when pressing the menu > |
||||
O( |
) to O( |
) |
||
8 |
LIST UPDATE |
Updates the list display. |
(Note 1) 1 to 7999 or 10000 to 99999999 can be set for the O No, and up to 18 alphanumeric characters can be set for the comment.
(Note 2) NC program mode includes user macro mode and MTB mode. (This is specified in the preferences screen.) When user macro mode is active and an NC program created with MTB mode is opened, the NC program is converted into user macro mode. When MTB mode is active and an NC program created with user macro mode is opened, the NC program is converted into MTB mode.
— 24 —
4. SCREEN SPECIFICATIONS
4.2 Screen Related to the Program |
||
Operation example (Opening the existing NC program) |
||
(1) |
The program edit screen will be displayed. |
|
Select the [PROGRAM] in the LIST |
||
VIEW area. |
The list of the NC program that can be read |
|
out will be displayed. |
||
(2)Press the [OPEN] menu key, and input the NC program No. to be read out.
The [OPEN] menu will be highlighted, and the setting area will be displayed.
(3)Press the [INPUT] key.
The highlight of the [OPEN] menu will turn OFF, and the setting area will disappear. The process of the NC program read out will be displayed in the LIST VIEW area. The NC program No. read out will be displayed on the area bar of the OPERATION VIEW area.
— 25 —
4. SCREEN SPECIFICATIONS
4.3 Screen Related to the Process Edit Functions
4.3 Screens Related to the Process Edit Functions
4.3.1 Process List Screen
The tool information and cutting conditions for each process are displayed on this screen. When [PROCESS] is selected in the LIST VIEW area, this screen is displayed.
When the NC program is not selected, this screen is not displayed.
Screen layout
Screen display items
No. |
Display item |
Details |
Setting range |
||||
1 |
PCS |
The process name is displayed. |
— |
||||
(Note) This name is same as the name displayed in |
|||||||
the LIST VIEW area. |
|||||||
2 |
T NAME |
The name of tool to be used is displayed. |
— |
||||
3 |
T |
The tool No. and compensation No. are displayed. |
0 to 99999999 |
||||
The tool No. can be changed. |
|||||||
T-command will not be output if the tool No. is set to |
|||||||
«0». Set the tool No. to «0» unless T-command |
|||||||
needs to be output, such as when the same tool is |
|||||||
used for the multiple consecutive processes. |
|||||||
4 |
V |
The cutting speed is displayed. |
1 to 9999 m/min |
||||
The cutting speed can be changed. |
1 to 9999 feet/min |
||||||
5 |
F |
The feedrate is displayed. The feedrate can be |
0.0001 to 999.9999 mm/rev |
||||
changed. When TAP or THREAD process is |
0.00001 to |
||||||
applied, the pitch (mm/rev) is displayed. |
99.99999 inch/rev |
||||||
Menus |
|||||||
No. |
Menu |
Details |
|||||
1 |
← |
Turns the LIST VIEW area active. |
|||||
2 |
SAVE |
Saves changes in the process list. |
— 26 —
4. SCREEN SPECIFICATIONS
4.3 Screen Related to the Process Edit Functions
4.3.2 Operating Process
When the cursor is moved to the sub-object of PROCESS in the LIST VIEW area, a menu for editing the process is displayed, and the process can be operated.
Screen layout
Menus
No. |
Menu |
Details |
1 |
MODIFY |
The OPERATION VIEW area turns active, and the process |
parameters can be changed. |
||
2 |
NEW |
Adds a new process. |
The process will be inserted into the cursor position. |
||
3 |
MOVE |
Changes the process position. |
4 |
DELETE |
Deletes the process at the cursor position. |
When performing the deletion, the process under the deleted process |
||
will be moved up. |
||
5 |
COPY |
Copies the process at the cursor position. |
The copied process will be inserted under the cursor position. |
||
— 27 —
4. SCREEN SPECIFICATIONS
4.3 Screen Related to the Process Edit Functions
Operation example (Selecting the process)
(1)Validate the LIST VIEW area, select the process with the cursor key.
The contents of the OPERATION VIEW area will change to those of the selected process.
(2)Press the [MODIFY] menu key.
The OPERATION VIEW area will turn active.
— 28 —
4. SCREEN SPECIFICATIONS
4.3 Screen Related to the Process Edit Functions
Operation example (Deleting the process)
(1)Validate the LIST VIEW area, select the process to be deleted with the cursor key.
The contents of the OPERATION VIEW area will change to those of the selected process.
(2)Press the [DELETE] menu key.
(3)Press the [Y] key.
When not deleting the process, press the [N] key
The [DELETE] menu will be highlighted, and a massage confirming the deletion will appear.
The highlight of the [DELETE] menu will turn OFF, and the process at the cursor position will be deleted.
The process under the deleted process will be moved up one.
The contents in the OPERATION VIEW area will change to those of the process at the cursor position.
— 29 —
4. SCREEN SPECIFICATIONS
4.3 Screen Related to the Process Edit Functions
Operation example (Copying the process)
(1)Validate the LIST VIEW area, select the process of the copy source with the cursor key.
The contents of the OPERATION VIEW area will change to those of the selected process.
(2)Press the [COPY] menu key.
The copied process will be inserted under the cursor position.
— 30 —
4. SCREEN SPECIFICATIONS
4.3 Screen Related to the Process Edit Functions
Operation example (Moving the process)
(1)Validate the LIST VIEW area, select the process to be moved with the cursor key.
The contents of the OPERATION VIEW area will change to those of the selected process.
(2)Press the [MOVE] menu key.
The [MOVE] menu will be highlighted. The mark «M» will be displayed beside the process to be moved.
(3)Select the position of the movement destination with the cursor key.
— 31 —
4. SCREEN SPECIFICATIONS
4.3 Screen Related to the Process Edit Functions
(4)Press the [INPUT] key.
If the [MOVE] menu key is pressed again during the movement operation, the movement operation will be canceled.
The message to confirm a movement is displayed.
(5)Press the [Y] key.
When not moving the process, press the [N] key
The process of the movement source will be moved to the cursor position.
The highlight of the [MOVE] menu will turn OFF.
(Note) For the [NEW] menu, refer to the next section.
— 32 —
4. SCREEN SPECIFICATIONS
4.3 Screen Related to the Process Edit Functions
4.3.3 Process Mode Selection Screen
When a new process is added, the process mode is selected on this screen.
Screen layout
• Turning process
• Milling Process
(Note) Milling process is available only when the milling interporation specifications are provided.
— 33 —
4. SCREEN SPECIFICATIONS
4.3 Screen Related to the Process Edit Functions
Screen display item
• Turning process
No. |
Display item |
Details |
Setting range |
||
1 |
Process mode |
Displays the process mode that can be selected for |
1: TURN |
||
the turning machining. |
2: COPY |
||||
Select the process mode by moving the sub cursor |
3: GROOVE |
||||
or inputting numerical values. |
4: T GROOVE |
||||
5: THREAD |
|||||
6: HOLE |
|||||
7: EIA |
|||||
• Milling Process |
|||||
No. |
Display item |
Details |
Setting range |
||
1 |
Process mode |
Displays the process mode that can be selected for |
1: MILL HOLE |
||
milling. |
2: KEYWAY |
||||
Select the process mode by moving the sub cursor |
3: CONTOUR |
||||
or inputting numerical values. |
|||||
Menu |
|||||
No. |
Menu |
Details |
|||
1 |
← |
Cancels adding a new process. |
|||
The LIST VIEW area will turn active after cancel. |
|||||
2 |
LATHE |
Displays the process mode for the turning machining. |
|||
(Note) This is valid when the milling interporation specifications are |
|||||
provided. |
|||||
3 |
MILLING |
Displays the process mode for milling. |
|||
(Note) This is valid when the milling interporation specifications are |
|||||
provided. |
— 34 —
4. SCREEN SPECIFICATIONS
4.3 Screen Related to the Process Edit Functions
Operation example (Adding a new process)
(1)Validate the LIST VIEW area, and select the position where the process is added with the cursor key.
(2)Press the [NEW] menu key.
Select turning mode or milling mode by pressing [LATHE] or [MILLING] respectively.
A blank process will be inserted into the cursor position.
The process mode selection screen will be displayed in the OPERATION VIEW area, and the OPERATION VIEW area will turn active.
(3)Select the process mode with the cursor or the numerical value input.
— 35 —
4. SCREEN SPECIFICATIONS
4.3 Screen Related to the Process Edit Functions |
|||
(4) |
The contents in the OPERATION VIEW |
||
Press the [INPUT] key. |
|||
area will change into those of the selected |
|||
process mode. |
|||
The selected process mode will be |
|||
displayed at the cursor position in the LIST |
|||
VIEW area. |
(Note) If the [←] menu key is pressed during adding the process, the screen will return to the state before pressing the [NEW] menu key (state of the 1).
— 36 —
Loading…