Page 1
Page 2
Page 3
MELDAS is registered trademarks of Mitsubishi Electric Corporation.
Other company and product names that appear in this manual are trademarks or registered trademarks of the respective
companies.
Page 4
Page 5
Introduction
CAUTION
This manual is a guide for using the MITSUBISHI CNC M700V/M70V 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
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 "no t 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 builde r 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 M700V/M70 Series Instruction Manual ............ IB-1500922
Page 6
Page 7
Precautions for Safety
WARNING
CAUTION
Always read the specifications issued by the machine tool builder, 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".
DANGER
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.
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.
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 unexpect ed 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 ax is 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 operato rs.
Page 8
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 opti on 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.
2. Items related to operation
Before starting actual machining, always carry out graphic check, dry ru n operation and single block
operation to check the machining program, tool compensation amount, workpiece compensation amount
and 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.
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.
3. Items related to programming
The commands with "no value after G" will be handled as "G00".
";" "EOB" and "%" "EOR" are expressions used for explanation. The actual codes are: For ISO: "CR, LF", or
"LF" and "%".
Programs created on the Edit screen are stored in the NC memory in a "CR, LF" fo rmat, but 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 build er .
When programming the multi-part system, take special care to the mov ements of the programs for other
part systems.
Page 9
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 manufact ured 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 sep arately
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!
Page 10
Page 11
CONTENTS
1 Control Axes .... ....................................... ... .... ... ... ... ....................................... ... ... .... ... ................................. 1
1.1 Coordinate Words and Control Axes ............................................................. .... ... ... ... .... ... ... ... .............. 2
1.2 Coordinate Systems and Coordinate Zero Point Symbols .................................................................... 3
2 Least Command Increments ........... ... ... ... .... ... ... ....................................... ... ... ... .... .................................... 5
2.1 Input Setting Unit ............................................. ... ....................................... ... .... ... ... ... ........................... 6
2.2 Input Command Increment Tenfold ....................................................................................................... 7
2.3 Indexing Increment ............................................................................................................................... 8
3 Program Formats ...................................... ....................................... ... .... ... ... ... ........................................... 9
3.1 Program Format ............................ ... ... .... ... ... ... ....................................... ... ... .... ... ............................... 10
3.2 File Format ................................. ... ... ... .... ... ... ....................................... ... ... ... .... .................................. 14
3.3 Optional Block Skip ............................................................................................................................. 16
3.3.1 Optional Block Skip; / ........ ... ... ... ....................................... ... .... ... ... ... ... ...................................... 16
3.3.2 Optional Block Skip Addition ; /n ................................................................................................. 17
3.4 G code .................................................... ... ....................................... ... ... ... ... .... .................................. 19
3.4.1 Modal, unmodal .......................................................................................................................... 19
3.4.2 G Code Lists................................................................................................................................ 19
3.5 Precautions Before Starting Machining ................... ...... ... .... ... ... ... .... ... ... ... ... .... ... ... ... .... ...... ... ............ 23
4 Pre-read Buffers ........... ... .... ... ... ... .... ...................................... .... ... ... ... ...................................................... 25
4.1 Pre-read Buffers ............................ ....................................... ... ... ... .... ... ............................................... 26
5 Position Commands ....... .... ... ... ....................................... ... ... .... ... ............................................................ 27
5.1 Position Command Methods ; G90,G91 .............................................................................................. 28
5.2 Inch/Metric Conversion ; G20,G21....................................................................................................... 30
5.3 Decimal Point Input ............................. .... ... ... ... ... .... ...................................... .... ... ... ... ......................... 32
6 Interpolation Functions ............................................................................................................................ 37
6.1 Positioning (Rapid Traverse) ; G00..................................................................................................... 38
6.2 Linear Interpolation ; G01 .................................................................................................................... 44
6.3 Circular Interpolation ; G02,G03......................................................................................................... 46
6.4 R Specification Circular Interpolation ; G02,G03 ................................................................................. 51
6.5 Plane Selection ; G17,G18,G19........................................................................................................... 53
6.6 Thread Cutting.................. ... ... .... ... ... ... .... ...................................... .... ... ... ... ... ...................................... 55
6.6.1 Constant Lead Thread Cutting ; G33............... ... ... ... .... ... ... ....... ... ... ... ... .... ... ... ... .... ... ... ... ... .... . .... 55
6.6.2 Inch Thread Cutting ; G33........................................................................................................... 60
6.7 Helical Interpolation ; G17 to G19, G02, G03 ...................................................................................... 62
6.8 Unidirectional positioning ; G60 ........................................................................................................... 67
6.9 Cylindrical Interpolation ; G07.1........................................................................................................... 68
6.10 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113 .............................................................. 75
6.11 Exponential Interpolation ; G02.3,G03.3............................................................................................ 82
6.12 Polar Coordinate Command ; G16..................... .... ... ... ... .... ... ....................................... ... ... ... ............ 88
6.13 Spiral/Conical Interpolation ; G02.0/G03.1(Type1), G02/G03(Type2)............................................... 95
6.14 3-dimensional Circular Interpolation ; G02.4,G03.4......................... ... ... ... ....... ... ... ... .... ... ... ... ... .... ...100
6.15 NURBS interpolation ; G06.2................................................. ... ... .... ................................................ 105
6.16 Hypothetical Axis interpolation ; G07............................................................................................... 110
7 Feed functions .................................. ...................................... .... ... ... ... .... ................................................ 113
7.1 Rapid Traverse Rate............................ .... ...................................... .... ... ... ... ... .................................... 114
7.2 Cutting Feedrate .................... .... ... ... ... ....................................... ... .... ... ... ... ..................
7.3 F1-digit
7.4 Feed Per Minute/Feed Per Revolution (Asynchronous Feed/Synchronous Feed) ; G94,G95 .......... 119
7.5 Inverse Time Feed ; G93......................... ... ....................................... ... ... ... ... .... ................................ 121
7.6 Feedrate Designation and Effects on Control Axes........................................................................... 126
7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration ....................................................... 131
Feed..................... ... ... .... ... ... ... .... ...................................... .... ... ... ... ... .................................... 116
..................... 115
Page 12
7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration ....................................... 133
7.9 Exact Stop Check ; G09..................................................................................................................... 142
7.10 Exact Stop Check Mode ; G61......................................................................................................... 146
7.11 Deceleration Check. ......................................................................................................................... 147
7.11.1 G1 -> G0 Deceleration Check.................................................................................................. 149
7.11.2 G1 -> G1 Deceleration Check.................................................................................................. 150
7.12 Automatic Corner Override ; G62..................................................................................................... 151
7.13 Tapping Mode ; G63 ........................................................................................................................ 157
7.14 Cutting Mode ; G64......................................................................................................................... 158
8 Dwell.......................................................................................................................................................... 159
8.1 Dwell (Time Designation) ; G04......................................................................................................... 160
9 Miscellaneous Functions ....................................................................................................................... 163
9.1 Miscellaneous Functions (M8-digits) ................................................................................................. 164
9.2 Secondary Miscellaneous Functions (A8-digits, B8-digits or C8-digits) ............................................ 166
9.3 Index Table Indexing ......................................................................................................................... 167
10 Spindle Functions.................................................................................................................................. 169
10.1 Spindle Functions................................. ... .... ... ... ... ... .... ...................................... .... ... ... .....................170
10.2 Constant Surface Speed Control ; G96,G97.................................................................................... 171
10.3 Spindle Clamp Speed Setting ; G92 ................................................................................................173
10.4 Spindle/C Axis Control...................................... ... ... .... ...................................... .... ... ... ... .................. 175
10.5 Multiple-spindle Control....................................................................................................................178
10.5.1 Multiple-spindle Control II ........................................................................................................ 179
11 Tool Functions (T command) ............................................................................................................... 181
11.1 Tool Functions (T8-digit BCD) .........................................................................................................182
12 Tool Compensation Functions ............................................................................................................ 183
12.1 Tool compensation........................................................................................................................... 184
12.2 Tool Length Compensation/Cancel ; G43,G44/G49 ........................................................................ 188
12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G49................................................. 191
12.4 Tool Radius Compensation ; G38,G39/G40/G41,G42..................................................................... 199
12.4.1 Tool Radius Compensation Operation................................................................... .... ... ... ... ... .. 200
12.4.2 Other Commands and Operations during Tool Radius Compensation.................................... 209
12.4.3 G41/G42 Commands and I, J, K Designation ......................................................................... 220
12.4.4 Interrupts during Tool Nose Radius Compensation ................................................................ 226
12.4.5 General precautions for tool radius compensation .................................................................. 229
12.4.6 Changing of Compensation No. during Compensation Mode.................................................. 230
12.4.7 Start of Tool Radius Compensation and Z Axis Cut in Operation............................................ 233
12.4.8 Interference Check ................... ... ....................................... ... ... .... ... ... ..................................... 235
12.4.9 Diameter Designation of C
12.4.10 Workpiece Coordinate Changing during Radius Compensation............................................246
12.5 3-dimensional Tool Radius Compensation ; G40/G41,G42. .... ... ... ....... ... ... ... ... .... ... ... ... .... ... ... ... ... .. 248
12.6 Tool radius compensation for 5-axis machining ; G40/G41.2,G42.2 ............................................... 259
12.7 Tool Position Offset ; G45 to G48.................................................................................................... 269
12.8 Programmable Compensation Input ; G10,G11... ... .... ... ... ... .... ...................................... .... ... ... ... ... .. 277
12.9 Inputting the Tool Life Management Data ; G10,G11 ...................................................................... 282
12.9.1 Inputting the Tool Life Management Data by G10 L3 Command ; G10 L3,G11...................... 282
12.9.2 Inputting the Tool Life Management Data by G10 L30 Command ; G10 L30,G11.................. 284
12.9.3 Precautions for Inputting the Tool Life Management Data............... ... ... ... .... ... ... ... .... ... ... ... ... .. 287
ompensation Amount..................................................................... 244
13 Program Support Functions ................................................................................................................ 289
13.1 Fixed cycles ...... ... ... ... ... ....................................... ... .... ... ... ... ............................................................ 290
13.1.1 Drilling, spot drilling ; G81........................................................................................................ 294
13.1.2 Drilling, counter boring ; G82 ...................................................................................................295
13.1.3 Deep hole drilling cycle ; G83.................................................................................................. 296
13.1.4 Tapping cycle ; G84................................................................................................................. 297
13.1.5 Boring ; G85.............................. ... ... .... ... ... ... ... ....................................... ... .... ... ... ... ..................308
Page 13
13.1.6 Boring ; G86............................................................................................................................. 309
13.1.7 Back boring ; G87.................................................................................................................... 310
13.1.8 Boring ; G88............................................................................................................................. 312
13.1.9 Boring ; G89............................................................................................................................. 313
13.1.10 Stepping cycle ; G73.............................................................................................................. 314
13.1.11 Reverse tapping cycle ; G74.................................................................................................. 315
13.1.12 Circular cutting ; G75............................................................................................................. 317
13.1.13 Fine boring ; G76................................................................................................................... 319
13.1.14 Precautions for using a fixed cycle ........................................................................................ 321
13.1.15 Initial Point and R Point Level Return ; G98,G99................................................................... 324
13.1.16 Setting of Workpiece Coordinates in Fixed Cycle Mode ....................................................... 325
13.1.17 Drilling Cycle with High-Speed Retract..................................................................................326
13.2 Special Fixed Cycle ............................................... ... ... ... .... ...................................... .... ................... 330
13.2.1 Bolt hole cycle ; G34................................................................................................................ 331
13.2.2 Line at angle ; G35 .................................................................................................................. 332
13.2.3 Arc ; G36.................................................................................................................................. 333
13.2.4 Grid ; G37.1 ............................................................................................................................. 334
13.3 Subprogram Control; M98, M99, M198 ........................................................................................... 335
13.3.1 Subprogram Call ; M98,M99................................................................................................... 335
13.3.2 Subprogram Call ; M198......................................................................................................... 340
13.3.3 Figure rotation ; M98 I_J_K_.................................................................................................... 341
13.4 Variable Commands ....................................................................................................................... 344
13.5 User Macro ............................................ ... ....................................... ... ... ... ... .... ................................ 348
13.5.1 User Macro ............................................................................................................................. 348
13.5.2 Macro Call Instruction ............................................................................................................. 349
13.5.2.1 Simple Macro Calls ; G65............................................................................................... 349
13.5.2.2 Modal Call A (Movement Command Call) ; G66............................................................. 352
13.5.2.3 Modal Call B (for each block) ; G66.1............................................................................. 354
13.5.2.4 G Code Macro Call ......................................................................................................... 355
13.5.2.5 Miscellaneous Command Macro Call (for M, S, T, B Code Macro Call) ......................... 356
13.5.2.6 Detailed Description for Macro Call Instruction .............................................................. 357
13.5.3 ASCII Code Macro .................................................................................................................. 359
13.5.4 Variable.................................................................................................................................... 363
13.5.5 Types of Variables .................................................................................................................. 365
13.5.5.1 Common Variables ......................................................................................................... 365
13.5.5.2 Local Variables (#1 to #33) ............................................................................................. 366
13.5.5.3 Macro Interface Inputs/Outputs
(#1000 to #1035, #1100 to #1135, #1200 to #1295, #1300 to #1395) ........................... 371
13.5.5.4 Tool Compensation ......................................................................................................... 378
13.5.5.5 Workpiece Coordinate System Compensation (#5201 - #532n) ..................................... 379
13.5.5.6 NC Alarm (#3000) ............................. .... ... ... ... .... ... ....................................... ... ... ... ... ....... 380
13.5.5.7 Integrating Time (#3001, #3002) .................................................................................... 381
13.5.5.8 Suppression of Single Block Stop and Miscellaneous Function Finish Signal Waiting
(#3003) ........................................................................................................................... 381
13.5.5.9 Feed Hold, Feedrate Override, G09 Valid/Invalid (#3004) ............................................. 382
13.5.5.10 Message Display and Stop (#3006) .............................................................................. 382
13.5.5.11 Mirror Image (#3007) .................................................................................................... 383
13.5.5.12 G Command Modals (#4001-#4021, #4201-#4221) ..................................................... 384
13.5.5.13 Other Modals (#4101 - #4120, #4301 - #4320) ............................................................ 385
13.5.5.14 Position Information (#5001 - #5140 + n) .... ....................................... ... .... ... ... ... .......... 386
13.5.5.15 Number of Workpiece Machining Times (#3901, #3902) ................................... ... .... ... 389
13.5.5.16 Coordinate rotation parameter
13.5.5.17 Rotary Axis Configuration Parameters .......................................................................... 390
13.5.5.18 Reverse run information ................................................................................................ 390
13.5.5.19 Tool Life Management (#60000 - #64700) ................................................................... 391
13.5.5.20 Reading The Parameters (#100000-#100002, #100010) ... ... ... .... ... ... ... .... ... ... ... ... .... ... 396
13.5.5.21 Reading PLC data (#100100-#100103,#100110) ............................ ............................. 400
13.5.5.22 Time Reading Variables (#3001, #3002, #3011, #3012) .............................................. 404
13.5.5.23 R Device Access Variables
(#50000 - #50749, #51000 - #51749, #52000 - #52749) .............................................. 406
13.5.5.24 Read/write of the workpiece installation error compensation amounts.......................... 412
....................................................................................... 389
Page 14
13.5.6 Operation Commands ........................ ...................................... .... ... ... ... ... ............................... 413
13.5.7 Control Commands .................................................. ... .... ... ... ... .... ........................................... 418
13.5.8 External Output Commands ; POPEN,PCLOS,DPRNT ......................................................... 421
13.5.9 Precautions . ...... ... .... ... ... ... .... ... ... ... .........................................................................................425
13.5.10 Actual examples of using user macros .................................................................................. 427
13.6 G command mirror image ; G50.1,G51.1................................. ... ... ... .... ...................................... ..... 431
13.7 Corner Chamfering/Corner Rounding I ........................................................................................... 435
13.7.1 Corner Chamfering I ; G01 X_ Y_ ,C...................................................................................... 435
13.7.2 Corner Rounding I ; G01 X_ Y_ ,R_ ....................................................................................... 437
13.8 Linear Angle Command ; G01 X_/Y_ A_/,A_...................................................................................439
13.9 Geometric ; G01 A_ ............ ... ....................................... ... ... .... ... ... .................................................. 440
13.10 Circular cutting ; G12,G13............................... ... ... .... ... ... ... ....................................... ... .................. 443
13.11 Programmable Parameter Input ; G10 L70/L50, G11.................................................................... 445
13.12 Macro Interruption ; M96,M97............... .... ... ... ... ....................................... ... ... .... ... ........................ 447
13.13 Tool Change Position Return ; G30.1 - G30.6.......................... ... ... .... ... ... ... .................................. 455
13.14 Normal line control ; G40.1/G41.1/G42.1........................................ .... ... ... ... ... .... ... ... ... .... ... ... ........ 458
13.15 High-accuracy control ; G61.1,G08....................... .... ... ....................................... ... ... ... .... ..............470
13.16 High speed machining mode.......................................................................................................... 485
13.16.1 High-speed Machining Mode I, II ; G05 P1, G05 P2..............................................................485
13.17 High-speed High-accuracy control ; G05, G05.1 ........................................................................... 487
13.17.1 High-speed high-accuracy control I, II ; G05.1 Q1/Q0,G05 P10000/P0 ................................487
13.17.2 SSS Control...........................................................................................................................493
13.18 Spline ; G05.1 Q2/Q0.. .... ...................................... .... ... ... ... .... ...................................... .................. 499
13.19 High-accuracy Spline Interpolation ; G61.2.................................................................................... 508
13.20 Scaling ; G50/G51..........................................................................................................................510
13.21 Coordinate rotation by program ; G68/G69.................................................................................... 514
13.22 Coordinate Rotation Input by Parameter ; G10 I_ J_/K_................................................................ 521
13.23 3-dimensional coordinate conversion ; G68/69..............................................................................524
13.24 Tool center point control ; G43.4/G43.5.........................................................................................539
13.25 Waiting-and-simultaneous Operation ; !L....................................................................................... 567
13.26 Inclined Surface Machining ; G68.2, G68.3 ...................................................................................570
13.26.1 How to Define Feature Coordinate System Using Euler Angles.... ... ... ... ....... ... ... .... ... ... ... ... .. 571
13.26.2 How to Define Feature Coordinate System Using Roll-Pitch-Yaw angles ............................. 572
13.26.3 How to Define Feature Coordinate System Using Three Points in a Plane........................... 574
13.26.4 How to Define Feature Coordinate System Using Two Vectors ............................................ 576
13.26.5 How to Define Feature Coordinate System Using Projection Angles .................................... 578
13.26.6 How to Define Feature Coordinate System Using Tool Axis Direction .................................. 580
13.26.7 Tool Axis Direction Control .................................................................................................... 582
13.26.8 Details of Operation ...................................................................................................
13.26.9 Rotary
13.26.10 Relation with other functions................................................................................................ 594
13.26.11 Precautions.............................................. ... .... ... ....................................... ... ... ... .................. 597
Axis Basic Position Selection ..................................................................................... 588
............ 584
14 Coordinate System Setting Functions................................................................................................. 601
14.1 Coordinate Words and Control Axes................................................................................................ 602
14.2 Basic Machine, Workpiece and Local Coordinate Systems . .... ... ... ... .... ... ... ... ... .... ... ... ... ....... ... ... ... .. 603
14.3 Machine Zero Point and 2nd, 3rd, 4th Reference Position (Zero point) ..........................................604
14.4 Automatic Coordinate System Setting ............................................................................................. 605
14.5 Basic Machine Coordinate System Selection ; G53......................................................................... 606
14.6 Coordinate System Setting ; G92..................................................................................................... 607
14.7 Reference Position (Zero point) Return ; G28,G29.......................................................................... 608
14.8 2nd, 3rd, and 4th Reference Position (Zero point) Return ; G30 ..................................................... 612
14.9 Reference Position Check ; G27.............................................. ... ... ... .... ... ........................................ 615
14.10 Workpiece Coordinate System Setting and Offset ; G54 to G59 (G54.1)...................................... 616
14.11 Local Coordinate System Setting ; G52........................................................................................ 627
14.12 Workpiece Coordinate System Preset ; G92.1 ............................................................................. 631
14.13 Coordinate System for Rotary Axis................................................................................................ 636
14.14 Workpiece Installation Error Compensation ; G54.4...................................................................... 639
15 Measurement Support Functions ........................................................................................................ 653
15.1 Automatic Tool Length Measurement ; G37 .................................................................................... 654
Page 15
15.2 Skip Function ; G31 .................................................... ... .... ... ... ....................................................... 658
15.3 Multi-step Skip Function 1 ; G31.n ,G04......................................................................................... 662
15.4 Multi-step Skip Function 2 ; G31 P ................................................................................................. 664
15.5 Speed Change Skip ; G31 Fn ........................................................................................................ 666
15.6 Programmable Current Limitation ; G10 L14 ;....................... ....................................... ... ... ... ... .... ... 670
15.7 Stroke Check Before Travel ; G22/G23........................................................................................... 671
Appendix 1 Program Errors....................................................................................................................... 673
Appendix 2 Order of G Function Command Priority ............................................................................... 705
Page 16
Page 17
1
1
Control Axes
Page 18
1 Control Axes
MITSUBISHI CNC
1.1 Coordinate Words and Control Axes
+Z
+Z
+Y
+X
+X
+Y
(a)
(a)
+Z
+Y
+C
+C
+Y
+X
+X
(a)
(b)
(a)
Function and purpose
In the standard specifications, there are 3 control axes, however, 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 coor dinate
word made up of alphabet characters that have been decided beforehand.
X-Y table
(a) Direction of table movement
X-Y and rotating table
(a) Direction of table movement (b) Direction of table rotation
2
Page 19
M700V/M70V Series Programming Manual (Machining Center System)
1.2 Coordinate Systems and Coordinate Zero Point Symbols
1.2 Coordinate Systems and Coordinate Zero Point Symbols
G52
Reference position:
A specific position to establish coordinate systems and change tools
Basic machine coordinate zero point:
A position specific to machine
Workpiece coordinate zero points (G54 to G59)
A coordinate zero point used for workpiece machining
The basic machine coordinate system is the coordinate system that expresses the position (tool change
position, stroke end position, etc.) that is specific to the machine.
Workpiece coordinate systems are used for workpiece machining.
Upon completion of the dog-type reference position return, the parameters are referred and the basic machine
coordinate system and workpiece coordinate systems (G54 to G59) are automatically set.
The offset of the basic machine coordinate zero point and reference position is set by a parameter. (Normally,
set by machine manufacturers)
Workpiece coordinate systems can be set with coordinate systems setting functions, workpiece coordinate
offset measurement (additional specification), and etc.
G54
G92
EXT
Reference position
Basic machine coordinate zero point
Workpiece coordinate zero points
Local coordinate zero point
G52
G55
G52 Local coordinate system offset (*1)
G54 Workpiece coordinate (G54) system offset (*1)
G55 Workpiece coordinate (G55) system offset
G92 G92 Coordinate system shift
EXT External workpiece coordinate offset
Offset set by a parameter
Offset set by a program
("0" is set when turning the power ON)
(*1) G52 offset is independently possessed by G 54
to G59 respectively.
The local coordinate systems (G52) are valid on the coordinate systems designated by workpiece coordinate
systems 1 to 6.
Using the G92 command, the basic machine coordinate system can be shifted and made into a hypothetical
machine coordinate system. At the same time, workpiece coordinate systems 1 to 6 are also shifted.
3
Page 20
1 Control Axes
MITSUBISHI CNC
4
Page 21
5
2
Least Command
Increments
Page 22
2 Least Command Increments
MITSUBISHI CNC
2.1 Input Setting Unit
Function and purpose
The input setting units are the units of setting data including tool compensation amounts and workpiece
coordinates compensation.
The program command units are the units of movement amounts in programs.
These are expressed with mm, inch or degree (°).
Detailed description
Program command units for each axis and input setting units, common for all axes, are determined by the
setting of parameters as follows.
Input setting unit
Program command
unit
Parameter
#1003 iunit = B 0.001 0.0001 0.001
= C 0.0001 0.00001 0.0001
= D 0.00001 0.000001 0.00001
= 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
= 10000 1.0 0.1 1.0
Linear axis
Millimeter Inch
Rotary axis
(°)
Precautions
(1) Inch/metric changeover can be handled by either a parameter screen (#1041 I_inch: valid only when the
power is turned ON) or G commands (G20 or G21).
However, the changeover by a G command applies only to the program command units, and not to the
input setting units. Consequently, the tool compensation amounts and other compensation amounts as
well as the variable data should be pr e s e t in order to correspond to input setting units.
(2) The millimeter and inch systems cannot be used together.
(3) When performing a circular interpolation between the axes whose program command units are different,
the center command (I, J, K) and the radius command (R) are designated by the input setting units. (Use
a decimal point to avoid confusion.)
6
Page 23
M700V/M70V Series Programming Manual (Machining Center System)
2.2 Input Command Increment Tenfold
2.2 Input Command Increment Tenfold
N1
N2
N3
N4
N5
R
-400
-300
-200
-100
W
-100-200-300
N6
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 10μm input command increment with a CNC
unit for which the command increment is set to 1μm and this function's parameter value is set to "10",
this function enables the same machining as the original program.
(2) When running a machining program already created with a 1μm input command increment with a CNC
unit for which the command increment is set to 0.1μm and this function's parameter value is set to "10",
this function enables the same machining as the original program.
(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.
(Machining program : programmed with 1=10μm)
Program example
(CNC unit is 1=1μm system)
"UNIT*10" parameter
10 1
XYXY
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 Y20.000 -180.000 -380.000 0.000 -20.000
-10-20-30
N6
N2
W
-10
-20
-30
-40
N1
N3
N4
N5
R
UNIT*10 ON UNIT*10 OFF
7
Page 24
2 Least Command Increments
MITSUBISHI CNC
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) which limits the command value is set, the rotary axis can only 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, the machine coordinate position at the end
point can only be commanded with the 2-degree increment.
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 Details Setting range (unit)
2106 Index unit
Indexing
increment
Set the indexing increment with which the rotary axis can be
positioned.
0 to 360(°)
Precautions
(1) When the indexing increment is set, positioning will be conducted in degree unit.
(2) The indexing position is checked with the rotary axis, and is not checked with other axes.
(3) 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 "G91B2." is
commanded.
8
Page 25
9
3
Program Formats
Page 26
3 Program Formats
MITSUBISHI CNC
3.1 Program Format
%
Block
Block
Block
Block
Block
Block
Block
Block
Block
%
A collection of commands assigned to an NC to move a machine is called "program".
A program is a collection of units called "block" which specifies a sequence of machine tool operations.
Blocks are written in the order of the actual movement of a tool.
A block is a collection of "words" which constitutes a command to an operation.
A word is a collection of characters (alphabets, numerals, signs) arranged in a specific sequence.
10
Page 27
M700V/M70V Series Programming Manual (Machining Center System)
3.1 Program Format
Detailed description
Program
A program format looks as follows.
(1)
(2)
(3)
(4)
(5)
%
O 㧧
(COMMENT)
Block
Block
Block
Block
Block
Block
Block
Block
%
(1) Program start
Input an End Of Record (EOR, %) at the head of a program.
It is automatically added when writing a program on an NC. When using an external device, do not forget
to input it at the head of a program. For details, refer to the description of the file format.
(2) Program No.
Program Nos. are used to classify programs by main program unit or subprogram unit. They are
designated by the address "O" followed by numbers of up to 8 digits. Program Nos. must be written at
the head of programs. A setting is available to prohibit O8000s and O9000s from editing (edit lock). Refer
to the instruction manual for the edit lock.
(3) Comment
Data between control out "(" and control in ")" is ignored.
Information including program names and comments can be written in.
(4) Program section
A program is a collection of several blocks.
(5) Program end
Input an end of record (EOR, %) at the end of a program.
It is automatically added when writing a program on an NC.
11
Page 28
3 Program Formats
MITSUBISHI CNC
Block and word
EOB
Word Word
Word
...
;
Word
(a) (n)
[Block]
A block is a least command increment, consisting of words.
It contains the information which is required for a tool machine to execute a specific operation. One block unit
constitutes a complete command.
The end of each block is marked with an End of Block (EOB, expressed as ";" for the sake of convenience).
[Word]
(a) Alphabet (address)
(n) Numerals
A word consists of a set of an alphabet, which is called an address, and numerals (numerical information).
Meanings of the numerical information and the number of significant digits of words differ according to an
address.
The major contents of a word are described below.
N_ _ _ G__ X _ _ Z__ F__ ;
(1) (2)
(1) Sequence No.
A "sequence No." consists of the address "N" followed by numbers of up to 6 digits (Normally 3 or 4
digits). It is used as an index when searching a necessary block in a program (as branch destination and
etc.).
It does not affect the operation of a tool machine.
(2) Preparatory functions (G code, G function)
"Preparatory function (G code, G function)" consists of the address G followed by numbers of 2 or 3
digits (it may include 1 digit after the decimal point). G codes are mainly used to designate functions,
such as axis movements and setting of coordinate systems. For example, G00 executes a positioning
and G01 executes a linear interpolation.
There are 6 types of G code systems, 2, 3, 4, 5, 6 and 7. Refer to the description of G code system for
available G codes.
(3) Coordinate words
"Coordinate words" specify the coordinate position and movement amounts of tool machine axes. They
consist of an address which indicates each axis of a tool machine followed by numerical information (+ or
- signs and numerals).
X, Y, Z, U, V, W, A, B and C are used as address. Coordinate positions and movement amounts are
specified by either "incremental value commands" or "absolute value commands".
(3)
(4) EOB
12
(4) Feed Functions (F functions)
"Feed Functions (F functions)" designate the speed of a tool relative to a workpiece. They consist of the
address F followed by numbers.
Page 29
M700V/M70V Series Programming Manual (Machining Center System)
3.1 Program Format
Main program and subprograms
(MP) (S1)
(S2)
O0010;
M98P1000;
M98P2000;
M02;
O1000;
M99;
O2000;
M99;
(MP) Main program
(S1) Subprogram 1
(S2) Subprogram 2
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.
If a command is issued to call a subprogram while a main program is being executed, the subprogram will be
executed. And when the subprogram is completed, the main program will be resumed.
Refer to the description of subprogram control for the details of the execution of subprograms.
13
Page 30
3 Program Formats
MITSUBISHI CNC
3.2 File Format
(COMMENT) ;
G28XYZ ;
M02 ;
%
Function and purpose
Program file can be created using NC edit screen and PC.
It can be input/output between NC memory and an external I/O device. Hard discs stored in NC unit are
regarded as an external I/O device. For the details of input/output method, refer to the instruction manual.
Program file format differs depending on the device which creates the program.
Detailed description
Devices available for input/output
Devices which can input/output program files are as follows.
NC memory
HD (internal hard disc) ○ --
Serial ○○○
Memory card (front IC card) ○○○
DS (NC control unit side compact flash) ○ --
FD ○ -USB memory - ○ -
Ethernet ○○○
Anshin-net server ○○○
External I/O device M700VW M700VS M70V
○○○
Program file format
The file format for each external I/O device is as follows.
(1) NC memory (Creates program on NC)
End of record (EOR, %)
Program No. (O No.) Not necessary.
File transfer
The end of record (EOR, %) is automatically added.
It does not need to be input purposely.
When multiple programs within the NC memory are transferred to an external device as serial, they will be integrated into one file in the external device.
When a file containing multiple programs in an external device is transferred to NC
memory as serial, it will be divided into one file per one program.
14
Page 31
M700V/M70V Series Programming Manual (Machining Center System)
3.2 File Format
(2) External device (except for serials, such as memory card, DS, FD, USB memory)
CRLF
CRLF
G28 XYZ
CRLF
:
:
M02
CRLF
O101(COMMENT1)
CRLF
:
M02
CRLF
%
^Z
O100(COMMENT)
[Single program] [Multiple programs]
CRLF
(COMMENT)
G28 XYZ
CRLF
CRLF
:
:
M02
CRLF
%
^Z
The first line (from % to LF, or CR LF) will be skipped. Also, the content after the
End of record (EOR, %)
second % will not be transferred.
"%" must be included in the first line because if not, the necessary information
when transferring a file to an NC memory cannot be transferred.
Program No. (O No.)
O No. before (COMMENT) will be ignored and the file name will be given the priority.
Transfer and check of multiple programs between external devices, except for serial <_> serial, are not available.
When a file containing multiple programs in an external device is transferred to NC
File transfer
memory as serial, it will be divided into one file per one program.
When transferring divided programs one by one from an external device, which is
not serial, (multiple programs) to an NC memory, the head program name can be
omitted like "(COMMENT)" only when the transferring destination file name is designated to the file name field of device B.
Program name
Program name should be designated with up to 32 alphanumeric characters (29
characters for a multi-part system program).
End of block (EOB, ;) When the I/O parameter "CR output" is set to "1", EOB becomes CRLF.
(3) External device (serial)
LF
%
O100(COMMENT)
G28 XYZ
LF
LF
:
:
M02
LF
%
The first line (from % to LF, or CR LF) will be skipped. Also, the content after the
End of record (EOR, %)
second % will not be transferred.
"%" must be included in the first line because if not, the necessary information
when transferring a file to an NC memory cannot be transferred.
Transfer and check of multiple programs between external devices, except for serial <_> serial, are not available.
File transfer
When transferring a file as serial, the head program name can be omitted like
"(COMMENT)" only when the transferring destination file name is designated to
the file name field of device B.
Program name
Program name should be designated with up to 32 alphanumeric characters (29
characters for a multi-part system program).
End of block (EOB, ;) When the I/O parameter "CR output" is set to "1", EOB becomes CRLF.
15
Page 32
3 Program Formats
MITSUBISHI CNC
3.3 Optional Block Skip
3.3.1 Optional Block Skip; /
Function and purpose
This function selectively ignores specific blocks in a machining program which starts with the "/" (slash) code.
Detailed description
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 blocks 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
(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 No. 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.
16
Page 33
M700V/M70V Series Programming Manual (Machining Center System)
3.3 Optional Block Skip
3.3.2 Optional Block Skip Addition ; /n
N4 N2
N2N3N4
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 , di ff ere nt 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 n signal is turned ON. For a block with the "/n" code inside the block (not at the head of the
block), the program is operated according to the value of the parameter "#1226 aux10/bit1" setting.
When the optional block skip n signal is OFF, th e block with "/n" is executed.
Program example
(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.
Part 1
Optional block skip 5 signal ON
N1 G54 ;
N2 G90 G81 X50. Z-20. R3. F100 ;
/5 N3 X30. ;
N4 X10. ;
N5 G80 ;
M02 ;
Part 2
Optional block skip 5 signal OFF
17
Page 34
3 Program Formats
MITSUBISHI CNC
(2) When two or more "/n" codes are commanded at the head of the same block, the block will be ignored if
either of the optional block skip n signals corresponding to the command is ON.
N01 G90 Z3. M03 S1000 ; (a) Optional block skip 1 signal ON
/1/2 N02 G00 X50. ;
/1/2 N03 G01 Z-20. F100 ;
/1/2 N04 G00 Z3. ;
/1 /3 N05 G00 X30. ; (b) Optional block skip 2 signal ON
/1 /3 N06 G01 Z-20. F100 ;
/1 /3 N07 G00 Z3. ;
/2/3 N08 G00 X10. ; (c) Optional block skip 3 signal ON
/2/3 N09 G01 Z-20. F100 ;
/2/3 N10 G00 Z3. ;
N11 G28 X0 M05 ;
N12 M02 ;
(Optional block skip 2.3 signal OFF)
N01 -> N08 -> N09 -> N10 -> N11 -> N12
(Optional block skip 1.3 signal OFF)
N01 -> N05 -> N06 -> N07 -> N11 -> N12
(Optional block skip 1.2 signal OFF)
N01 -> N02 -> N03 -> N04 -> N11 -> N12
(3) When the parameter "#1226 aux10/bit1" is "1"and 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 n signals
corresponding to the command is ON.
N01 G91 G28 X0.Y0.Z0.; N03 block will operate as follows.
N02 G01 F1000;
N03 X1. /1 Y1. /2 Z1.;
N04 M30;
(a) Optional block skip 1 signal ON
Optional block skip 2 signal OFF
"Y1. Z1." is ignored.
(b) Optional block skip 1 signal OFF
Optional block skip 2 signal ON
"Z1." is ignored.
18
Page 35
M700V/M70V Series Programming Manual (Machining Center System)
3.4 G code
3.4 G code
3.4.1 Modal, unmodal
G codes define the operation modes of each block in programs.
G codes can be modal or unmodal command.
Modal commands always designate one of the G codes in the group as the NC operation mode. The
operation mode is maintained until a cancel command is issued or other G code among the same group is
commanded.
An unmodal command designates the NC operation mode only when it is issued. It is invalid for the next
block.
3.4.2 G Code Lists
G code Group Function Section
Δ 00 01 Positioning 6.1
Δ 01 01 Linear interpolation 6.2
02 01
03 01
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
05 00
05.1 00
06.2 01 NURBS interpolation 6.15
07 00 Hypothetical axis inter polation 6.16
07.1
107
08 00 High-accuracy control 13.15
09 00 Exact stop check 7.9
10 00
11 00 Program data input cancel
12 00 Circular cut CW (clockwise) 13.10
13 00 Circular cut CCW (counterclockwise) 13.10
12.1
112
* 13.1
113
14
* 15 18 Polar coordinate command OFF 6.12
16 18 Polar coordinate command ON 6.12
Δ 17 02 Plane selection X-Y 6.5
Δ 18 02 Plane selection Z-X 6.5
Circular interpolation CW (clockwise)
R-specified circular interpolation CW
Helical interpolation CW
Spiral/Conical interpolation CW (type 2)
Circular interpolation CCW (counterclockwise)
R-specified circular interpolation CCW
Helical interpolation CCW
Spiral/Conical interpolation CCW (type 2)
Dwell
Multi-step skip function 1
High-speed machining mode
High-speed high-accuracy control II
High-speed high-accuracy control I
Spline
21 Cylindrical interpolation 6.9
Program data input (parameter /compensation data/parameter coordinate rotation data)
21 Polar coordinate interpolation ON 6.10
21 Polar coordinate interpolation cancel 6.10
6.3
6.4
6.7
6.13
6.3
6.4
6.7
6.13
8.1
13.16
13.17
13.17
13.18
12.8
13.11
13.22
12.8
13.11
19
Page 36
3 Program Formats
MITSUBISHI CNC
G code Group Function Section
Δ 19 02 Plane selection Y-Z 6.5
Δ 20 06 Inch command 5.2
Δ 21 06 Metric command 5.2
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
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 6.6
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
41 07
42 07
* 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
41.2 07 Tool radius compensation for 5-axis machining (left) 12.6
42.2 07 Tool radius compensation for 5-axis machining (right) 12.6
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) 12.7
46 00 Tool position offset (reduction) 12.7
47 00 Tool position offset (doubled) 12.7
48 00 Tool position offset (halved) 12.7
* 49 08
Skip
Multi-step skip function 2
Tool radius compensation cancel
3-dimentional tool radius compensation cancel
Tool radius compensation for 5-axis machining cancel
Tool radius compensation left
3-dimentional tool radius compensation left
Tool radius compensation right
3-dimentional tool radius compensation right
Tool length compensation cancel
Tool length compensation in the tool axis direction
Tool center point control cancel
15.2
15.4
12.4
12.5
12.6
12.4
12.5
12.4
12.5
12.2
12.3
13.24
20
Page 37
M700V/M70V Series Programming Manual (Machining Center System)
3.4 G code
G code Group Function Section
* 50 11 Scaling cancel 13.20
51 11 Scaling ON 13.20
* 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 14.5
53.1 00 Tool axis direction control 13.26
* 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
54.4 27 Workpiece installation error compensation 14.14
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 13.5.2.1
66 14 User macro modal call A 13.5.2.2
66.1 14 User macro modal call B 13.5.2.3
* 67 14 User macro modal call cancel 13.5.2
68 16
68.2 16 Inclined surface machining command 13.26
68.3 16
* 69 16
70 09 User fixed cycle
71 09 User fixed cycle
72 09 User fixed cycle
73 09 Fixed cycle (step) 13.1.10
74 09 Fixed cycle (reverse tap) 13.1.11
75 09 Fixed cycle (circle cutting cycle) 13.1.12
76 09 Fixed cycle (fine boring) 13.1.13
77 09 User fixed cycle
78 09 User fixed cycle
79 09 User fixed cycle
* 80 09 Fixed cycle cancel 13.1
81 09 Fixed cycle (drill/spot drill) 13.1.1
82 09 Fixed cycle (drill/counter boring) 13.1.2
83 09 Fixed cycle (deep drilling) 13.1.3
84 09 Fixed cycle (tapping) 13.1.4
85 09 Fixed cycle (boring) 13.1.5
86 09 Fixed cycle (boring) 13.1.6
87 09 Fixed cycle (back boring) 13.1.7
88 09 Fixed cycle (boring) 13.1.8
Coordinate rotation by program ON
/ 3-dimensional coordinate conversion mode ON
Inclined surface machining command (Define using tool axis direction)
Coordinate rotation by program cancel
/ 3-dimensional coordinate conversion mode OFF
/ Inclined surface machining command cancel
13.21
13.23
13.26
13.21
13.23
13.26
21
Page 38
3 Program Formats
MITSUBISHI CNC
G code Group Function Section
CAUTION
89 09 Fixed cycle (boring) 13.1.9
Δ 90 03 Absolute value command 5.1
Δ 91 03 Incremental command value 5.1
92 00 Coordinate system setting / Spindle clamp speed setting 14.6
92.1 00 Workpiece coordinate system pre-setting 14.12
93 05 Inverse time feed 7.5
Δ 94 05 Feed per minute (Asynchronous feed) 7.4
Δ 95 05 Feed per revolution (Synchronous feed) 7.4
Δ 96 17 Constant surface speed control ON 10.2
Δ 97 17 Constant surface speed control OFF 10.2
* 98 10 Fixed cycle Initial level return 13.1.15
99 10 Fixed cycle R point level return 13.1.15
100 - 225 00 User macro (G code call) Max. 10 13.5.2
Precautions
(1) Codes marked with * are codes that must be or are selected in the initial state.
The codes marked with Δ are codes that should be or are selected in the initial state by the
parameters.
(2) If two or more G codes from the same code are commanded, the latter G code will be valid.
(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.
(4) Whether the modal is initialized or not depends on each reset input.
(a) "Reset 1"
The modal is initialized when the reset initial parameter "#1151 rstinit" turns ON.
(b) "Reset 2" and "Reset & rewind"
The modal is initialized when the signal is input.
(c) Resetting when emergency stop is canceled
Follows "Reset 1".
(d) When modal is automatically reset at the start of individual functions such as reference position
return.
Follows "Reset & rewind".
22
1. The commands with "no value after G" will be handled as "G00".
Page 39
M700V/M70V Series Programming Manual (Machining Center System)
3.5 Precautions Before Starting Machining
3.5 Precautions Before Starting Machining
CAUTION
1. 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.
2. Before starting actual machining, always carry out graphic check, dry run operation and
single block operation to check the machining program, tool compensation amount,
workpiece offset amount and etc.
23
Page 40
3 Program Formats
MITSUBISHI CNC
24
Page 41
25
4
Pre-read Buffers
Page 42
4 Pre-read Buffers
MITSUBISHI CNC
4.1 Pre-read Buffers
Function and purpose
During automatic processing, the contents of one block ahead 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.
Detailed description
The specifications of pre-read buffers in 1 block are as follows:
(1) The data of 1 block is stored in this buffer.
(2) When comments 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.
(3) The pre-read buffer contents are cleared with resetting.
(4) When the single block function is ON during continuous operation, the pre-read buffer stores the next
block's data and then stops operation.
(5) The way to prohibit the M command which operates the external controls from pre-reading, and to make
it to recalculate, is as follows:
Identify the M command which operates the external controls by a PLC, and turn on the "recalculation
request" on PLC output signal. (When the "recalculation request" is turned ON, the program that has
been pre-read is recalculated.)
Precautions
(1) Depending on whether the program is executed continuously or by single blocks, the timing of the
validation/invalidation of the external control signals including optional block skip, 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 for the program pre-read with the buffer register.
26
Page 43
27
5
Position Commands
Page 44
5 Position Commands
MITSUBISHI CNC
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
G90/G91 X__ Y__ Z__ α__ ;
G90 Absolute command
G91 Incremental command
X,Y,Z,α Coordinate values (α is the additional axis.)
28
Page 45
M700V/M70V Series Programming Manual (Machining Center System)
5.1 Position Command Methods ; G90,G91
Detailed description
300.
200.
200.
100
N1
100.
N2
W
X
Y
300.
200.100.
N4
W
X
Y
100.
200.
(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.
N1 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.
N2 G90 G01 X200. Y50. F100 ;
N2 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.
Tool
(2) For the next block, the last G90/G91 command that was given becomes the modal.
(G90) N3 X100. Y100. ;
The axis moves to the workpiece coordinate system X = 100.mm
and Y = 100.mm position.
(G91) N3 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.
Y
200.
100.
100.
W
N3
200.
X
300.
(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.
N4 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.
29
Page 46
5 Position Commands
MITSUBISHI CNC
5.2 Inch/Metric Conversion ; G20,G21
Function and purpose
The commands can be changed between inch and metric with the G20/G21 command.
Command format
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. It is invalid for rotation axes.
Output unit, command unit and setting unit
The counter, parameter setting and display unit are determined by parameter "#1041 I_inch". 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
Item
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
(metric internal unit)
#1041 I_inch=0
G21 G20 G21 G20
Initial inch ON
(inch internal unit)
#1041 I_inch=1
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
30
Page 47
M700V/M70V Series Programming Manual (Machining Center System)
5.2 Inch/Metric Conversion ; G20,G21
Precautions
(1) The parameter and tool data will be input/output with the unit set by "#1041 I_inch".
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 codes.
Command in a separate block.
- G05 (High-speed machining mode)
- G7.1 (Cylindrical Interpolation)
- G12.1 (Polar coordinate interpolation)
31
Page 48
5 Position Commands
MITSUBISHI CNC
5.3 Decimal Point Input
Function and purpose
This function enables to input decimal points. It assigns the decimal point in millimeter or inch units for the
machining program input information that defines the tool paths, distances and speeds.
Use the parameter "#1078 Decpt2" to select whether minimum input command increment (type I) or zero point
(type II) to apply to 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 I and type II, the values of the data commands without the decimal points are
shown in the table below.
Command Command unit Type I Type II
cunit=10000
cunit= 1000 100 1
X1;
cunit= 100 10 1
cunit= 10 1 1
1000
(μm, 10
-4
inch,10-3°)
1
(mm, inch, °)
(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)
Input unit
[mm]
Input unit
[inch]
Movement command
(linear)
-99999.999 to
99999.999
-9999.9999 to
9999.9999
Movement command
(rotary)
-99999.999 to
99999.999
Feedrate Dwell
0.001 to
10000000.000
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 (1μm, 10μm,
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.
32
Page 49
M700V/M70V Series Programming Manual (Machining Center System)
5.3 Decimal Point Input
Decimal point input I, II and decimal point command validity
Decimal point input I and II will result as follows when decimal points are not used in an address which a
decimal point command is valid. Whether an address is valid or invalid for the decimal point command is
shown in the table below.
Both decimal point input I and II will produce the same result when a command uses a decimal point.
(1) Decimal point input I
The least significant digit of command data matches the command unit.
(Example) When "X1" is commanded in 1μm system, the same result occurs as for an "X0.001"
command.
(2) Decimal point input II
The least significant digit of command data matches the command unit.
(Example) When "X1" is commanded in 1μm system, the same result occurs as for an "X1." command.
-Addresses used, validity of decimal point commands-
I
Decimal Point
Command
Valid Coordinate position data
Invalid Revolving table
Invalid Miscellaneous function code
Valid Angle data
Invalid Data settings, axis numbers (G10)
Valid Coordinate position data
Invalid Revolving table
Invalid Miscellaneous function code
Valid Coordinate position data
Invalid Revolving table
Invalid Miscellaneous function code
Valid Corner chamfering amount ,c
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
Inch thread: number of ridges,
precision thread: lead
Valid Feedrate, automatic tool length measurement speed
Valid Thread lead
Valid Number of Z axis pitch in synchronous tap
Invalid Tool length compensation number
Invalid Sequence numbers in subprograms
Invalid Programmable parameter input: bit type data
Invalid Basic spindle selection
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
Valid Coordinates for arc center and 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
Address
A
B
C
D
E Valid
F
G Valid Preparatory function code
H
J
Application Remarks
33
Page 50
5 Position Commands
MITSUBISHI CNC
Address
K
L
M Invalid Miscellaneous function codes
N
O Invalid Program numbers
P
Q
R
S
T Invalid Tool function codes
U Valid Coordinate position data
V Valid Coordinate position data
W Valid Coordinate position data
X
Y Valid Coordinate position data
Decimal Point
Command
Valid Coordinates for arc center and 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
Invalid Number of fixed cycle and subprogram repetitions
Invalid
Invalid Programmable parameter input: data setting selection L70
Invalid Programmable parameter input: 2-word type data 4 bytes
Invalid Tool life data
Invalid Sequence numbers
Invalid Programmable parameter input: data numbers
Invalid/Valid Dwell time Parameter
Invalid Subprogram program call: program No.
Invalid/Valid Dwell at tap cycle hole base Parameter
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 Programmable 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.
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
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
Invalid Spindle function codes
Invalid Maximum spindle clamp speed
Invalid Constant surface speed control: surface speed
Invalid Programmable parameter input: word type data 2 bytes
Valid Coordinate position data
Valid Dwell time
Program tool compensation input/workpiece offset input:
type selection
Application Remarks
L2, L20, L10, L11
L12, L13,
34
Page 51
M700V/M70V Series Programming Manual (Machining Center System)
5.3 Decimal Point Input
Address
Z Valid Coordinate position data
Decimal Point
Command
Application Remarks
(Note 1) Decimal poin ts are all valid in user macro arguments.
Program example
(1) Program example of decimal point valid address
Program example
G0 X123.45
(decimal points are all mm points)
G0 X12345
#111=123 #112=5.55
X#111 Y#112
#113=#111+#112
(addition)
#114=#111-#112
(subtraction)
#115=#111*#112
(multiplication)
#116=#111/#112
#117=#112/#111
(division)
X123.450 mm X123.450 mm X123.450 mm
X12.345 mm
(last digit is 1μm unit)
X123.000 mm
Y5.550 mm
#113=128.550 #113=128.550 #113=128.550
#114=117.450 #114=117.450 #114=117.450
#115=682.650 #115=682.650 #115=682.650
#116=22.162
#117=0.045
Decimal point command 1 Decimal point
When 1 = 10μm When 1 = 10μm
X123.450 mm X12345.000 mm
X123.000 mm
Y5.550 mm
#116=22.162
#117=0.045
When 1 = 1mm
X123.000 mm
Y5.550 mm
#116=22.162
#117=0.045
command 2
Precautions
(1) If an arithmetic operator is inserted, the data will be handled as data with a decimal point.
(Example1) G00 X123+0 ;
This is the X axis command 123mm command. It will not be 123μm.
35
Page 52
5 Position Commands
MITSUBISHI CNC
36
Page 53
37
6
Interpolation Functions
Page 54
6 Interpolation Functions
MITSUBISHI CNC
6.1 Positioning (Rapid Traverse) ; G00
CAUTION
Function and purpose
This command is accompanied by coordinate words and performs high-speed positioning of a tool, from the
present point (start point) to the end point specified by the coordinate words.
Command format
G00 X__ Y__ Z__α__ ; ... Positioning (Rapid Traverse)
X, Y, Z, α
The command addresses are valid for all additional axes.
Represent coordinates, and could be either absolute values or incremental values, depending on the setting of G90/G91. (α is the additional axis)
Detailed description
(1) Positioning will be performed at the rapid traverse rate set in the parameter "#2001 rapid".
(2) G00 command belongs to the 01 group and is modal. When G00 command is successively issued, the
following blocks can be specified only by the coordinate words.
(3) In the G00 mode, acceleration and deceleration are always carried out at the start point and end point of
the block. Before advancing to the next block, a commanded deceleration or an in-position check is
conducted at the end point to confirm that the movement is completed.
(4) G functions (G72 to G89) in the 09 group are cancelled (G80) by the G00 command.
1. The commands with "no value after G" will be handled as "G00".
38
Page 55
M700V/M70V Series Programming Manual (Machining Center System)
6.1 Positioning (Rapid Traverse) ; G00
Tool path
300
(mm)
(E)
(S)
fy=6400mm/min
Y
X
200
fx=9600mm/min
Whether the tool moves along a linear or non-linear path can be selected by the parameter "#1086 G0Intp".
The positioning time does not change according to the path.
(1) Linear path: When the parameter "#1086 G0Intp" is set to "0"
In positioning, a tool follows the shortest path which connects the start point and the end point. 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 X-axis and Y-axis rapid traverse rates are both 9600mm/min;
G91 G00 X-300000 Y200000 ; (With an input setting unit of 0.001mm)
The tool will follow the path shown in the figure below.
(S) Start point
(E) End point
(fx) Actual X axis rate
(fy) Actual Y axis rate
(2) Non-linear path: When the parameter "#1086 G0Intp" is set to "1"
In positioning, 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 X-axis and Y-axis rapid traverse rates are both 9600mm/min;
G91 G00 X-300000 Y200000 ; (With an input setting unit of 0.001mm)
The tool will follow the path shown in the figure below.
(E)
200
Y
X
fy=9600mm/min
(S) Start point
(E) End point
(fx) Actual X axis rate
(fy) Actual Y axis rate
(S)
300
fx=9600mm/min
(mm)
39
Page 56
6 Interpolation Functions
MITSUBISHI CNC
Program example
mm
( - 120,+200,+300)
(+150, - 100,+150)
X
Z
Y
+300
+150
+200
+150
-100
- 120
(S)
(E)
G91 G00 X-270. Y300. Z150. ;
(S) Start point
(E) End point
Precautions for deceleration check
There are two methods for the deceleration check; commanded deceleration method and in-position check
method. Select a method with the parameter "#1193 inpos".
A block with an in-position width command performs an in-position check with a temporarily changed inposition width. (Programmable in-position width command)
The deceleration check method set in basic specification parameter "#1193 inpos" is used for blocks that do
not have the in-position width command.
When the error detection is ON, the in-position check is forcibly carried out.
Rapid traverse (G00)
,I command
Cutting feedrate
,I command
No
Yes In-position check method (In-position check by ",I", "#2077 G0inps", "#2224 SV024")
(G01)
No
Yes In-position check method (In-position check by ",I", "#2078 G1inps", "#2224 SV024")
Commanded deceleration method (Commanded deceleration check which varies according to the type of acceleration/
deceleration, set in "#2003 smgst" bit3-0)
Commanded deceleration method (Commanded deceleration check which varies according to the type of acceleration/
deceleration, set in "#2003 smgst" bit7-4)
01
01
* Following descriptions are for the case of rapid traverse. For G01, interpret the parameters into suitable
ones.
#1193 inpos
In-position check method (In-position check by
"#2077 G0inps", "#2224 SV024")
#1193 inpos
In-position check method (In-position check by
"#2078 G1inps", "#2224 SV024")
40
Page 57
M700V/M70V Series Programming Manual (Machining Center System)
6.1 Positioning (Rapid Traverse) ; G00
Commanded deceleration method when "inpos" = "0"
Td Ts
G00 Xx1; G00 Xx2;
2×Ts
Ts
Td
G00 Xx1; G00 Xx2;
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 set in the
parameter "#2003 smgst".
(1) Linear acceleration/linear deceleration
G00 Xx1; G00 Xx2;
Ts
Td
(Ts) Acceleration/deceleration time constant (Td) Deceleration check time: Td = Ts + (0 to 7ms)
(2) Exponential acceleration/linear deceleration
(Ts) Acceleration/deceleration time constant (Td) Deceleration check time: Td = 2 × Ts + (0 to 7ms)
(3) Exponential acceleration/exponential deceleration (Primary delay)
(Ts) Acceleration/deceleration time constant (Td) Deceleration check time: Td = 2 × Ts + (0 to 7ms)
The time required for the deceleration check is the longest among the deceleration check times of each axis
determined by the acceleration/deceleration mode and time constants of the axes commanded
simultaneously.
41
Page 58
6 Interpolation Functions
MITSUBISHI CNC
In-position check method when "inpos" = 1
SV024
(a)
(b)
G0inps
A
G0inps
(a)
(b)
SV024
A
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.
The confirmation of the remaining distance should be done with the imposition width.
The bigger one of the servo parameter "#2224 SV024" or G0 in-position width "#2077 G0inps" (For G01, inposition width "#2078 G1inps"), will be adapted as the in-position width.
The purpose of the rapid traverse deceleration check is to minimize the positioning time. The bigger the
setting value for the in-position width, the shorter the time is, but the remaining distance of the previous block
at the start 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
effect of time reduction for positioning as in-position width setting value.
(1) In-position check by the G0inps: When SV024 < G0inps (Stop is judged at A in the figure)
(a) Command to motor
(b) Outline of motor movement
(2) In-position check using SV024: When G0inps < SV024 (Stop is judged at A in the figure)
42
(a) Command to motor
(b) Outline of motor movement
Page 59
M700V/M70V Series Programming Manual (Machining Center System)
6.1 Positioning (Rapid Traverse) ; G00
Programmable in-position width command
This command commands the in-position width for the positioning command from the machining program.
G00 X_ Y_ Z_ ,I_ ;
X,Y,Z Positioning coordinate value of each axis
,I In-position width
Execution of the next block starts after confirming that the position error amount of the positioning (rapid
traverse: G00) command block is less than the in-position width issued in this command.
The bigger one of in-position width (SV024, G0inps (For G01, G1inps)) with parameter or in-position width
specified by program will be adapted as the in-position width.
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 In-position check
The differences between the in-position check with parameter and with programmable command are as
follows:
(1) In-position check with parameter
After completing deceleration of the command system (A), the servo system's position error amount and
the parameter setting value (in-position width) are compared.
(a)
(b)
(c)
(a) Servo machine position
G00 Xx1;
Ts
(b) Command
(c) In-position width (Servo system position error amount)
(Ts) Acceleration/deceleration time constant
(Td) Deceleration check time: Td = Ts + (0 to 7ms)
Td
A
(2) In-position check with programmable command (",I" address command)
After starting deceleration of the command system (A), the position error amount and commanded inposition width are compared.
(a)
G00 Xx1;
Ts
(b)
(c)
(a) Servo machine position
(b) Command
(c) In-position width (Error amount between command end point and
machine position)
(Ts) Acceleration/deceleration time constant
(Td) Deceleration check time: Td = Ts + (0 to 7ms)
Td
A
43
Page 60
6 Interpolation Functions
MITSUBISHI CNC
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 current 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__ α__ F__ ,I__ ; ... Linear interpolation
Coordinate values (α is the additional axis.)
X,Y,Z,α
F Feedrate (mm/min or °/min)
,I
Detailed description
An absolute position or incremental position is indicated based on the state of G90/G91 at
that time.
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. 1 to 999999 (mm)
(1) G01 command is a modal command in the 01 group. When G01 command is issued in succession, it can
only be issued with coordinate words in subsequent blocks.
(2) The feedrate for a rotary axis is commanded by °/min (decimal point position unit). (F300=300°/min)
(3) The G functions (G72 to G89) in the 09 group are cancelled (G80) by the G01 command.
Programmable in-position width command for linear interpolation
This command commands the in-position width for the linear interpolation command from the machining
program.
G01 X_ Y_ Z_ F_ ,I_ ;
X,Y,Z Linear interpolation coordinate value of each axis
F Feedrate
,I In-position width
The commanded in-position width is valid in the linear interpolation command only when carrying out
deceleration check.
- When the error detection switch is ON.
- When G09 (exact stop check) is commanded in the same block.
- When G61 (exact stop check mode) is selected.
(Note 1) Refer to section "Pos itioning (Rapid Traverse); G00" for details on the in-position check operation.
44
Page 61
M700V/M70V Series Programming Manual (Machining Center System)
6.2 Linear Interpolation ; G01
Program example
(Example) Cutting in the sequence of P1 -> P2 -> P3 -> P4 -> P1 at 300mm/min feedrate.
However, P0 -> P1 is for tool positioning.
Y
30
P2
P3
30
P1
20
20
P4
20
P0
G91 G00 X20. Y20. ; P0 -> P1
G01 X20. Y30. F300 ; P1 -> P2
X30. ; P2 -> P3
X-20. Y-30. ; P3 -> P4
X-30. ; P4 -> P1
X
45
Page 62
6 Interpolation Functions
MITSUBISHI CNC
6.3 Circular Interpolation ; G02,G03
Function and purpose
These commands serve to move the tool along a circular.
Command format
G02 X__ Y__ I__ J__ F__ ; ... Circular interpolation : Clockwise (CW)
G03 X__ Y__ I__ J__ F__ ; ... Circular interpolation : Counterclockwise (CCW)
X,Y End point
I,J Arc center
F Feedrate
46
Page 63
M700V/M70V Series Programming Manual (Machining Center System)
6.3 Circular Interpolation ; G02,G03
Detailed description
G02
G03
X
Z
(1) 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
circular command of an axis for which the program command unit (#1015 cunit) differs. Command with a
decimal point to avoid confusion.
(2) G02 (G03) is a modal command of the 01 group. When G02 (G03) command is issued continuously, the
next block and after can be commanded with only coordinate words.
The circular rotation direction is distinguished by G02 and G03.
G02 Clockwise (CW)
G03 Counterclockwise (CCW)
Z
G3
G3
G2
G3
Y
Z
G03
G02
Y
G2
G2
X
Y
G03
G02
X
G17(X-Y) plane G18(Z-X) plane G19(Y-Z) plane
(3) An arc which extends for more than one quadrant can be executed with a single block command.
(4) 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) Circular end point coordinates : Given by addresses X, Y, Z
(d) Circular center coordinates : Given by addresses I, J, K (incremental value commands)
(e) Feedrate : Given by address F
47
Page 64
6 Interpolation Functions
MITSUBISHI CNC
Plane selection
N1
N3
20
0
The arc exists in the following three planes (refer to the figure in the “Detailed description”), and are selected
by 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 operated up to the end point coordinate value only for that
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"
G90 X0 Y0 ;
N1 G02 X20. I10. F500 ; ... (a)
N2 G00 X0 ;
N3 G02 X20. F500 ; ... (b)
M02 ;
(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.
48
Page 65
M700V/M70V Series Programming Manual (Machining Center System)
6.3 Circular Interpolation ; G02,G03
Program example
F = 500mm/min
+Y
+X
J = 50mm
Y
X
(S) / (E)
(J)
F = 500mm/min
+Y
+X
J = 50mm
X50Y50mm
(J)
Y
X
(E)
(S)
(Example 1)
G02 J50. F500; Circle command
(S) Start point
(E) End point
(J) Circle center
(Example 2)
G91 G02 X50.Y50. J50. F500; 3/4 command
(S) Start point
(E) End point
(J) Circle center
49
Page 66
6 Interpolation Functions
MITSUBISHI CNC
Precautions
(G91) G02 X9.899 I5. ;
∆R
(S)
(AL)
(SR)
(ER)
(CP) (E)
(G91) G02 X9.9 I5. ;
∆R
(SI)
(E)
(CP)
(S)
(SR) (ER)
(1) The terms "clockwise" (G02) and "counterclockwise" (G03) used for circular operations are defined as a
case where, in a right-hand coordinate system, the negative direction is viewed from the positive
direction of the coordinate axis which is at right angles to the plane in question.
(2) If all the end point coordinates are omitted or the end point is at the same position as the start point,
commanding the center using I, J and K is the same as commanding a 360°arc (perfect circle).
(3) The following occurs when the start and end point radius do not match in a circular command :
(a) Program error (P70) occurs at the circular start point when error ΔR is greater than parameter "#1084 RadErr".
#1084 RadErr Parameter value 0.100
Start point radius=5.000
End point radius=4.899
ErrorΔR=0.101
(S) Start point
(CP) Center
(E) End point
(SR) Start point radius
(ER) End point radius
(AL) Alarm stop
(b) Spiral interpolation in the direction of the commanded end point will be conducted when error ΔR is less than the
parameter value.
#1084 RadErr Parameter value 0.100
Start point radius=5.000
End point radius=4.900
ErrorΔR=0.100
(S) Start point
(CP) Center
(E) End point
(SR) Start point radius
(ER) End point radius
(SI) Spiral interpolation
50
Page 67
M700V/M70V Series Programming Manual (Machining Center System)
6.4 R Specification Circular Interpolation ; G02,G03
6.4 R Specification Circular Interpolation ; G02,G03
L
1
2
r
Function and purpose
Along with the conventional circular interpolation commands based on the circular center coordinate (I, J, K)
designation, these commands can also be issued by directly designating the circular radius R.
Command format
G02 X__ Y__ R__ F__ ; ... R specification circular interpolation Clockwise (CW)
G03 X__ Y__ R__ F__ ; ... R specification circular interpolation Counterclockwise (CCW)
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 unit differs. Command with a decimal point to avoid confusion.
Detailed description
The circular center is on the bisector line which is perpendicular to the line connecting the start and end points
of the circular. The point, where the circular with the specified radius whose start point is the center intersects
the perpendicular bisector line, serves as the center coordinates of the circular command.
If the R sign of the commanded program is plus, the circular is smaller than a semicircular; if it is minus, the
circular is larger than a semicircular.
R < 0
(E)
(S) Start point
(E) End point
R > 0
L
(S)
The following condition must be met with an R-specified arc interpolation command:
r
When L/2 - r > parameter (#1084 RadErr), an alarm will occur.
Where L is the line from the start point to the end point. If an R specification and I, J, (K) specification are
given at the same time in the same block, the circular command with the R specification takes precedence. In
the case of a full-circle command (where the start and end points coincide), an R specification circular
command will be completed immediately even if it is issued and no operation will be executed. An I, J, (K)
specification circular command should therefore be used in such a case.
51
Page 68
6 Interpolation Functions
MITSUBISHI CNC
Circular center coordinate compensation
When the error margin between “the segment connecting the start and end points" and "the co mmanded
radius × 2" is less than the setting value, "the midpoint of segment connecting the start and end points" is
compensated as the circular center, because the required semicircle is not obtained by calculation error in R
specification circular interpolation.
Set the setting value to the parameter "#11028 Tolerance Arc Cent (Tolerable correction value of arc center
error)".
(Example) "#11028 Tolerance Arc Cent" = "0.000 (mm)"
Setting value Tolerance value
Setting value < 0 0(Center error will not be interpolated)
Setting value = 0 2×minimum setting increment
Setting value > 0 Setting value
G90 X0 Y0 ;
N1 G02 X10. R5.000;
N1, N3
N5
N2 G0 X0; ...(a)
N3 G02 X10. R5.001;
N4 G0 X0; ...(b)
N5 G02 X10. R5.002;
N6 G0 X0;
M02 ;
010
(a) Compensate the center coordinate: Same as N1 path
(b) Do not compensate the center coordinate: Slightly inside N1 path
Calculation error margin compensation allowance value: 0.002 mm
Segment connecting the start and end points: 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.
Program example
(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)
XY plane R-specified arc
G02 Xx1 Yy1 Ii1 Jj1 Rr1 Ff1 ;
(Example 4)
(When the R specification and I, J, (K) specification are contained
in the same block, the circular command with the R specification
takes precedence.)
G17 G02 Ii1 Jj1 Rr1 Ff1 ;
52
XY plane
This is an R-specified arc, but as this is a circle command, it will
be completed immediately.
Page 69
M700V/M70V Series Programming Manual (Machining Center System)
6.5 Plane Selection ; G17,G18,G19
6.5 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.
If the 3 basic axes and the parallel axes corresponding to these basic axes are entered as parameters, the
commands can select the plane composed of any 2 axes which are not parallel axes. If a rotary axis is
registered as a parallel axis, the commands can select the plane containing the rotary axis.
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 ; ... Plane selection X-Y
G18 ; ... Plane selection Z-X
G19 ; ... Plane selection Y-Z
X, Y and Z indicate each coordinate axis or th e parallel axis.
Detailed description
Parameter entry
#1026-1028base_I,J,K #1029-1031aux_I,J,K
IX U
JY
KZ V
Table 1 Examples of plane selection parameter entry
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.
53
Page 70
6 Interpolation Functions
MITSUBISHI CNC
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) Axis addresses assigned in the same block as the plane selection (G17, G18, G19) command determine
which of the basic axes or parallel axes are to be in the actual plane selected.
For the parameter entry example in Table 1.
G17 X__Y__ ; XY plane
G18 X__V__ ; VX plane
G18 U__V__ ; VU plane
G19 Y__Z__ ; YZ plane
G19 Y__V__ ; YV plane
(2) The plane will not changeover at a block where a plane selection G code (G17, G18, G19) is not
commanded.
G17 X__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 is assumed that the axis addresses of the 3 basic axes have been omitted.
For the parameter entry example in Table 1.
G17 ; XY plane
G17 U__ ; UY plane
G18 U__ ; ZU plane
G18 V__ ; VX plane
G19 Y__ ; YZ plane
G19 V__ ; 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 entry example in Table 1.
G17 U__Z__ ;
If the above is commanded, the UY plane will be selected, and Z will move regardless of the plane.
(5) When the basic axes or their parallel axes are duplicated and assigned in the same block as the plane
selection G code (G17, G18, G19), the plane is determined in the order of basic axes, and then parallel
axes.
For the parameter entry example in Table 1.
G17 U__Y__W__ ;
If the above is commanded, the UY plane will be selected, and W will move regardless of the plane.
(Note 1) When the power is turned ON or when the system is reset, the plane set by the parameters "#1025
I_plane" is selected.
54
Page 71
M700V/M70V Series Programming Manual (Machining Center System)
6.6 Thread Cutting
6.6 Thread Cutting
6.6.1 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__ α__) F__ Q__ ; ... Normal lead thread cutting
Z (X Y α) Thread end point
F Lead of long axis (axis which moves the most) direction
Q Thread cutting start shift angle (0.001 - 360.000°)
G33 Z__(X__ Y__ α__) E__ Q__ ; ... Precision lead thread cutting
Z (X Y α) Thread end point
E Lead of long axis (axis which moves most) direction
Q Thread cutting start shift angle (0.001 - 360.000°)
55
Page 72
6 Interpolation Functions
MITSUBISHI CNC
Detailed description
LZ
Z
X
LX
a
(t)
(1) The E command is also used for the number of ridges in inch thread cutting, and whether the number of
ridges or precision lead is to be designated can be selected by parameter setting.(Parameter "#1229 set
01/bit" is set to "1" for precision lead designation.)
(2) The lead in the long axis direction is commanded for the taper thread lead.
(t) Tapered thread section
When a < 45°, lead is in Z-axis direction.
When a < 45°, lead is in X-axis direction.
When a = 45°, lead can be in either Z or X-axis direction.
Thread cutting metric input
Input set-
ting unit
Command
address
Least
Command
Increments
Command
range
Input set-
ting unit
Command
address
Least
Command
Increments
Command
range
B (0.001mm) C (0.0001mm)
F (mm/rev) E (mm/rev) E (ridges/inch) F (mm/rev) E (mm/rev) E (ridges/inch)
1(=1.000)
(1.=1.000)
0.001 -
999.999
F (mm/rev) E (mm/rev) E (ridges/inch) F (mm/rev) E (mm/rev) E (ridges/inch)
1(=1.00000)
(1.=1.00000)
0.00001 -
999.99999
1(=1.0000)
(1.=1.0000)
0.0001 -
999.9999
D (0.00001mm) E (0.000001mm)
1(=1.000000)
(1.=1.000000)
0.000001 -
999.999999
1(=1.00)
(1.=1.00)
0.03 -
999.99
1(=1.0000)
(1.=1.0000)
0.0255 -
224580.0000
1(=1.0000)
(1.=1.0000)
0.0001 -
999.9999
1(=1.000000)
(1.=1.000000)
0.000001 -
999.999999
1(=1.00000)
(1.=1.00000)
0.00001 -
999.99999
1(=1.0000000)
(1.=1.0000000)
0.0000001 -
999.9999999
1(=1.000)
(1.=1.000)
0.026 -
222807.017
1(=1.00000)
(1.=1.00000)
0.02541 -
224719.00000
56
Page 73
M700V/M70V Series Programming Manual (Machining Center System)
6.6 Thread Cutting
Thread cutting inch input
Input set-
ting unit
Command
address
Least
Command
Increments
Command
range
Input set-
ting unit
Command
address
Least
Command
Increments
Command
range
F (inch/rev) E (inch/rev) E (ridges/inch) F (inch/rev) E (inch/rev) E (ridges/inch)
1(=1.0000)
(1.=1.0000)
0.0001 -
39.3700
F (inch/rev) E (inch/rev) E (ridges/inch) F (inch/rev) E (inch/rev) E (ridges/inch)
1(=1.000000)
(1.=1.000000)
0.000001 -
39.370078
B (0.0001inch) C (0.00001inch)
1(=1.00000)
(1.=1.00000)
0.00001 -
39.37007
D (0.000001inch) E (0.0000001inch)
1(=1.0000000)
(1.=1.0000000)
0.0000001 -
39.3700787
1(=1.000)
(1.=1.000)
0.025 -
9999.999
1(=1.00000)
(1.=1.00000)
0.02541 -
9999.99999
1(=1.00000)
(1.=1.00000)
0.00001 -
39.37007
1(=1.0000000)
(1.=1.0000000)
0.0000001 -
39.3700787
1(=1.000000)
(1.=1.000000)
0.000001 -
39.370078
1(=1.00000000)
(1.=1.00000000)
0.00000001 -
39.37007873
1(=1.0000)
(1.=1.0000)
0.0255 -
9999.9999
1(=1.000000)
(1.=1.000000)
0.025401 -
9999.999999
(Note 1) It is not possible to assign a lead where the feedrate as converted into feed per minute exceeds the
maximum cutting feedrate.
(3) The constant surface speed control function should not be used for taper thread cutting commands or
scrolled thread cutting commands.
(4) The spindle rotation speed should be kept constant throughout from the rough cutting until the finishin g.
(5) 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 occur at the end point of the block
following the block in which thread cutting is completed (no longer G33 mode).
(6) 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 occur.
(7) In order to protect the lead during thread cutting, a cutting feedrate which has been converted may
sometimes exceed the cutting feed clamp rate.
(8) 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.
(9) The spindle rotation speed is subject to the following restriction :
1 <= R <= Maximum feed rate/Thread lead
Where R <= Tolerable speed of encoder (r/min)
R: Spindle rotation 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.)
(10) A program error (P97) may occur when the result of the expression (9) is R<1 because the thread lead is
very large to the highest cutting feedrate.
(11) Dry run is valid for thread cutting but the feedrate 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.
(12) Synchronous feed applies for the thread cutting commands even with an asynchronous feed command
(G94).
57
Page 74
6 Interpolation Functions
MITSUBISHI CNC
(13) Spindle override and cutting feed override are invalid and the speeds are fixed to 100% during thread
cutting.
(14) When a thread cutting command is commanded during tool radius compensation, the compensation is
temporarily canceled and the thread cutting is executed.
(15) 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.
(16) 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 (G33 mode
is cancelled) is first executed and then the automatic operation stops. Note that automatic operation is
stopped until the G33 command axis starts moving.
(17) The thread cutting command waits for the single rotation synchronization signal of the rotary encoder
and starts movement.
Make sure to carry out waiting-and-simultaneous operation between part systems before issuing a
thread cutting command with multiple part systems. For example, when using 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 synchronization signal causing an illegal operation.
(18) The thread cutting start shift angle is not modal. If there is no Q command with G33, this will be handled
as "Q0".
(19) The automatic handle interrupt/interruption is valid during thread cutting.
(20) If a value exceeding 360.000 is command in G33 Q, a 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.
58
Page 75
M700V/M70V Series Programming Manual (Machining Center System)
6.6 Thread Cutting
Program example
Z
X
Y
X
10
50
10
N110 G90 G0 X-200. Y-200. S50 M3 ;
N111 Z110. ;
N112 G33 Z40. F6.0 ;
N113 M19 ; Spindle orientation is executed with the M19 command.
N114 G0 X-210. ; The tool is evaded in the X axis direction.
N115 Z110. M0 ;
N116 X-200. ;
M3 ;
N117 G04 X5.0 ; Command dwell to stabilize the spindle rotation if necessary.
N118 G33 Z40. ; The second thread cutting is executed.
The spindle center is positioned to the workpiece center, and the spindle
rotates in the forward direction.
The first thread cutting is executed.
Thread lead = 6.0mm
The tool rises to the top of the workpiece, and the program stops with M00.
Adjust the tool if required.
Preparation for second thread cutting is done.
59
Page 76
6 Interpolation Functions
MITSUBISHI CNC
6.6.2 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 threadcutting and tapered thread-cutting can be performed.
Command format
G33 Z__ E__ Q__ ; ... Inch thread cutting
Z Thread cutting direction axis address (X, Y, Z, α ) and thread length
E
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 number of ridges or
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 converted to lead.
(4) See Section "Constant lead thread cutting" for other details.
Number of ridges per inch in direction of long axis (axis which moves most) (decimal point command can also be assigned)
60
Page 77
M700V/M70V Series Programming Manual (Machining Center System)
6.6 Thread Cutting
Program example
Z
X
Y
X
1
50.0mm
2
Thread lead ..... 3 threads/inch (= 8.46666 ...)
When programmed with δ1= 10 mm, δ2=10 mm using metric input
N210 G90 G0 X-200. Y-200. S50 M3 ;
N211 Z110. ;
N212 G91 G33 Z-70. E3.0 ; (First thread cutting)
N213 M19 ;
N214 G90 G0 X-210. ;
N215 Z110. M0 ;
N216 X-200. ;
M3 ;
N217 G04 X2.0 ;
N218 G91 G33 Z-70. ; (Second thread cutting)
61
Page 78
6 Interpolation Functions
MITSUBISHI CNC
6.7 Helical Interpolation ; G17 to G19, G02, G03
Y
Z
X
F'
F
Y
X
(E)
(S)
(S)
(E)
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.
(S) Start point (E) End point
Command format
G17/G18/G19 G02/G03 X__ Y__ Z__ I__ J__ P__ F__ ; ... Helical interpolation command (Specify arc
center)
G17/G18/G19 G02/G03 X__ Y__ Z__ R__ F__ ; ... Helical interpolation command (Specify radius (R))
G17/G18/G19 Arc plane (G17: X-Y plane, G18: Z-X plane, G19: Y-Z plane)
G02/G03 Arc rotation direction (G02: clockwise, G03: counterclockwise)
X, Y Arc end point coordinates
Z Linear axis end point coordinates
I, J Arc center coordinates
P Number of pitches
R Arc radius
F Feedrate
The arc center coordinate value and arc radius value are commanded with an input setting unit. 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 coordin ates.
The arc plane element speed designation and normal speed designation can be sele cted with the parameter.
#1235 set07/bit0 Meaning
1 Arc plane element speed designation is selected.
0 Normal speed designation is selected.
62
Page 79
M700V/M70V Series Programming Manual (Machining Center System)
6.7 Helical Interpolation ; G17 to G19, G02, G03
Detailed description
L =
= e- s =tan
-1
-tan
-1
()0 <2
ys
ye
xs
xe
(2
P1+ )/2
Z
1
Normal speed designation
Y
Z
e
P
1
(E)
Z
Y
2
1
1
L
X
(S) Start point (E) End point
(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.
s
(S)
X
(2) For feedrate F, command the X, Y and Z axis composite element directions speed.
(3) Pitch L is obtained with the following expression.
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.
63
Page 80
6 Interpolation Functions
MITSUBISHI CNC
(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.
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 G17 (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 "Plane Selection" for the arc planes selected with these command
methods.
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.
(Example)
G17 G91 G02 X10. Y10. Z-4. I10. F100 ;
G01 X20. ; Linear interpolation at F100
G02 X10. Y-10. Z4. J10. ;
G01 Y-40. F120; Linear interpolation at F120
G02 X-10. Y-10. Z-4. I10. ;
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.
Helical interpolation at speed at which arc plane element is
F100
Helical interpolation at speed at which arc plane element is
F100
Helical interpolation at speed at which arc plane element is
F120
64
Page 81
M700V/M70V Series Programming Manual (Machining Center System)
6.7 Helical Interpolation ; G17 to G19, G02, G03
Program example
z1
Z
Y
X
z1
r1
Z
Y
X
z1
Z
Y
U
(Example 1)
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.
(Example 2)
G17 ; XY plane
G02 Xx1 Yy1 Zz1 Rr1 Ff1; XY plane arc, Z axis linear
(Example 3)
G17 G03 Uu1 Yy1 Zz1 Ii1 Jj1 P2 Ff1; UY plane arc, Z axis linear
65
Page 82
6 Interpolation Functions
MITSUBISHI CNC
(Example 4)
u1
z1
x1
Z
X
U
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;
(Note) Two or more axes can be designated for the linear interpolation axis.
ZX plane arc, U axis, Y axis linear
(The J command is ignored)
66
Page 83
M700V/M70V Series Programming Manual (Machining Center System)
6.8 Unidirectional positioning ; G60
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 constant direction.
Command format
G60 X__ Y__ Z__ α__; ... Unidirectional positioning
α Additional 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 moves to the final positio n in accordance with the rapid
traverse setting where its positioning is completed.
G60a
(PP)
(FD)
-
(S)
(ST)
(S) Start point (E) End point (ST) Stop once
(PP) Positioning position (FD) Final advance direction (CD) G60 creep 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 stop 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) Unidirectional positioning is not performed for the drilling ax is during drilling fixed cycles.
(8) Unidirectional 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.
(19) Unidirectional 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) will occur when the G60 command is assigned with an NC system which has not
been provided with this particular specification.
(E)
G60- a
(CD)
(S)
+
67
Page 84
6 Interpolation Functions
MITSUBISHI CNC
6.9 Cylindrical Interpolation ; G07.1
r
B
Z
X
Y
0
360
2 r
Function and purpose
This function develops a shape on the side of a cylinder (shape in a cylindrical coordinate system) into a
plane. When the developed shape is programmed as the plane coordinates, it will be converted into a linear
axis movement and rotary axis movement in the cylindrical coordinates to conduct a contour control when
machining.
As programming can be carried out to the developed shape of the side of the cylinder, this is effective for
machining cylindrical cams, etc. When programmed with the rotary axis and its orthogonal axis, grooves and
other shapes can be machined on the side of the cylinder.
Command format
G07.1 C__ ; ... Cylindrical interpolation mode start/cancel
Cylinder radius value (When rotary axis name is "C")
C
- Radius value ≠ 0: Cylindrical interpolation mode start
- Radius value = 0: Cylindrical interpolation mode cancel
68
Page 85
M700V/M70V Series Programming Manual (Machining Center System)
6.9 Cylindrical Interpolation ; G07.1
Detailed description
(1) The coordinate commands 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)
:
:
:
G07.1 C0 ; Cylindrical interpolation mode cancel (Cylindrical interpolation will be canceled)
(The coordinate commands in this interval will be the cylindrical coordinate system)
(2) G107 can be used instead of G07.1.
(3) Command G07.1 is an independent block. A program error (P33) will occur if this command is issued in
the same block as other G codes.
(4) Program the rotary axis with an angle degree.
(5) 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.
(6) The coordinate commands can be both an absolute command or incremental command.
(7) Tool radius compensation can be applied on the program command. Cylindrical interpolation will be
executed to the path after it has gone through a tool radius compensation.
(8) Command the tangent speed on the developed cylinder by F. F is in mm/min or inch/min unit.
Cylindrical interpolation accuracy
In the cylindrical interpolation mode, the movement amount of the rotary axis commanded with an angle is
converted into distance on a circle periphery, and after calculating 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 gap generated by this will not be cumulated.
Related parameters
#1516 mill_ax (Milling axis name)
#8111 Milling Radius
#1267 ext03/bit0 (G code type)
#1270 ext06/bit7 (Handling of C axis coordinate during cylindrical interpolation)
69
Page 86
6 Interpolation Functions
MITSUBISHI CNC
Plane selection
G17
Y
X
G18
Z
X
G19
Y
Z
G19
C
Z
G17
X
C
G18
C
X
G19
Y
C
G17
Y
X
G18
Z
X
G19
Y
Z
Z
C
G19
The axis used for cylindrical interpolation must be set with the plane selection command. (Note)
Use parameters (#1029, #1030 and #1031) to set which parallel axis corresponds to the rotary axis.
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 a movement
command is issued without this command, a program error (P485) will occur.
(Example)
G19 Z0. C0. ;
G07.1 C100. ;
:
G07.1 C0 ;
Basic coordinate system
X,Y,Z
Y
C
Cylindrical coordinate system
C , Y , Z
(Rotary axis is X axis' parallel
axis)
G17
G18
#1029
C
Z
Cylindrical coordinate system
X , C , Z
(Rotary axis is Y axis' parallel
axis)
#1030
Cylindrical coordinate system
X , Y , C
(Rotary axis is Z axis' parallel
axis)
#1031
(Note) Depending on the model or version, the Z-C plane (Y-Z cylindrical 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
70
Page 87
M700V/M70V Series Programming Manual (Machining Center System)
6.9 Cylindrical Interpolation ; G07.1
Program example
<Program>
N01 G28 XZC ;
N02 T020 ;
N03 G97 S100 M23 ;
N04 G00 X50. Z0. ;
N05 G94 G01 X40. F100. ;
N06 G19 C0 Z0 ; .......................................... . Plane selection command for cylindrical interpolation and two
axes command for interpolation
N07 G07.1 C20. ; .......................................... Cylindrical interpolation start
N08 G41 ;
N09 G01 Z-10. C80. F150 ;
N10 Z-25. C90. ;
N11 Z-80. C225 ;
N12 G03 Z-75.C270. R55. ;
N13 G01 Z-25 ;
N14 G02 Z-20.C280. R80. ;
N15 G01 C360. ;
N16 G40 ;
N17 G07.1 C0 ; ........................................... Cylindrical interpolation cancel
N18 G01 X50. ;
N19 G0 X100. Z100. ;
N20 M25 ;
N21 M30 ;
<Parameter>
#1029 aux_I
#1030 aux_J C
#1031 aux_K
N11
N12
N13
-20-40-60-80
N14
N15
N09N10
(mm)
Z
50
100
150
200
250
300
350
C
71
Page 88
6 Interpolation Functions
MITSUBISHI CNC
Relation with other functions
Circular interpolation
(1) Circular interpolation between the rotary axis and linear axis is possible during the cylindrical
interpolation mode.
(2) An R specification command can be issued with circular interpolation. (I, J and K cannot be designated.)
Tool radius compensation
The tool radius can be compensated during the cylindrical interpolation mode.
(1) Command the plane selection in the same manner as circular interpolation.
When using tool radius compensation, start up/cancel the compensatio n in the cylindrical interpolation
mode.
(2) A program error (P485) will occur if G07.1 is commanded during tool radius compensation.
(3) If the G07.1 command is issued with no movement command 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.
Cutting feed per minute (asynchronous feed)
(1) The feed per minute (asynchronous) mode is forcibly set when the cylindrical interpolation mode is
started.
(2) When the cylindrical interpolation mode is canceled, the feed per revolution (synchronous) will return to
the state before the cylindrical interpolation mode was started.
Constant surface speed control
(1) A program error (P485) will occur if G07.1 is commanded in the constant surface speed control mode
(G96).
Miscellaneous functions
(1) The miscellaneous function (M) and 2nd miscellaneous function can be issued in the cylindrical
interpolation mode.
(2) The S command in the cylindrical interpolation mode specifies the rotary tool's rotation speed instead of
the spindle rotation speed.
72
Page 89
M700V/M70V Series Programming Manual (Machining Center System)
6.9 Cylindrical Interpolation ; G07.1
Tool length compensation
(1) Program error (P481) will occur if tool length compensation is performed in the cylindrical interpolation
mode.
:
:
G43 H12 ;
G0 X100. Z0. ;
G19 Z C ;
G07.1 C100. ;
:
G43 H11 ;
:
G07.1 C0 ;
... Tool length compensation before cylindrical interpolation -> Valid
... Tool length compensation in cylindrical interpolation mode -> Program error
(2) Complete the tool compensation operation (movement of tool length and wear compensation amount)
before executing the cylindrical interpolation.
If the tool compensation operation is not completed when the cylindrical interpolation start command is
issued, the followings will occur:
- The machine coordinate will not change even if G12.1 is executed.
- The workpiece coordinate will change to that of the post tool length compensation when G07.1 is
executed.
(Even if the cylindrical interpolation is canceled, this workpiece coordinate will not be canceled. )
F command during cylindrical interpolation
As for the F command during cylindrical interpolation mode, whether to use the previous F command depends
on the previous mode of the feed per minute command (G94/G98) or feed per rotation command (G95/G99).
(1) When G94 (G98) is commanded just before G07.1
If there is no F command in the cylindrical interpolation, the previous F command feedrate will be used.
After the cylindrical interpolation mode is canceled, the F co mmand feedrate set at the start of the
cylindrical interpolation mode or the last F command feedrate set during cylindrical interpolation will
continue to be the feedrate.
(2) When G95 (G99) 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.
After the cylindrical interpolation mode is canceled, the feedrate will return to the state 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 With 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.
73
Page 90
6 Interpolation Functions
MITSUBISHI CNC
Restrictions and precautions
(1) The following G code commands can be used during the cylindrical interpolation mode.
G code Details
G00 Positioning
G01 Linear interpolation
G02 Circular interpolation (CW)
G03 Circular interpolation (CWW)
G04 Dwell
G09 Exact stop check
G40-42 Tool radius compensation
G61 Exact stop mode
G64 Cutting mode
G65 Macro call (simple call)
G66 Macro modal call (modal call)
G66.1 Macro modal call (block call per macro)
G67 Macro modal call cancel (modal call cancel)
G80-89 Fixed cycle for drilling
G90/91 Absolute/incremental value command
G94 Asynchronous feed
G98 Hole drilling cycle initial return
G99 Hole drilling cycle R point return
A program error will occur if a G code other than those listed above is commanded during cylindrical
interpolation.
(2) The cylindrical interpolation mode is canceled when the power is turned ON or reset.
(3) A program error (P484) will occur if any axis commanded during cylindrical interpolation has not
completed the reference position return.
(4) Tool radius compensation must be canceled before canceling the cylindric al interpolation mode.
(5) When the cylindrical interpolation mode is canceled and switched to the cutting mode, the plane selected
before the cylindrical interpolation will be restored.
(6) Program cannot be restarted (program restart) when the block is in the cylindrical interpolation.
(7) A program error (P486) will occur if the cylindrical interpolation command is issued during the mirror
image.
(8) When the cylindrical interpolation mode is started or canceled, the deceleration check is performed.
(9) A program error (P481) will occur if the cylindrical interpolation or the polar coordinate interpolation is
commanded during the cylindrical interpolation mode.
74
Page 91
M700V/M70V Series Programming Manual (Machining Center System)
6.10 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113
6.10 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113
X
C
Z
(c)
(a)
(b)
Function and purpose
This function converts the commands programmed with the orthogonal coordinate axis into linear axis
movement (tool movement) and rotary 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 "polar coordinate interpolation plane") is selected. Polar coordinate
interpolation is carried out on this plane. The workpiece coordinate system zero point is used as the
coordinate system zero point during polar coordinate interpolation.
(a) Linear axis (b) Rotary axis (hypothetical axis) (c) Polar coordinate interpolation plane (G17 plane)
This is effective for cutting a notch in a linear line to the external diameter of the workpiece, for cutting cam
shafts and etc.
Command format
G12.1; ... Polar coordinate interpolation mode start
G13.1; ... Polar coordinate interpolation mode cancel
75
Page 92
6 Interpolation Functions
MITSUBISHI CNC
Detailed description
(1) The coordinate commands in the interval from the start to cancellation of the polar coordinate
interpolation mode will be the polar coordinate interpolation.
G12.1; Polar coordinate interpolation mode start (Polar coordinate interpolation will start)
:
:
:
G13.1; Polar coordinate interpolation mode cancel (Polar coordinate interpolation is canceled)
(2) G112 and G113 can be used instead of G12.1 and G13.1.
(3) 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 other G codes.
(4) Linear interpolation or circular interpolation can be commanded during the polar coordinate interpolation
mode.
(5) The coordinate commands can be both an absolute command or incremental command.
(6) Tool radius compensation can be applied on the program command. Polar coordinate interpolation will
be executed to the path after it has gone through a tool radius compensation.
(7) Command the tangent speed in the polar coordinate interpolation plane (orthogonal coordinate system)
by F. F is in mm/min or inch/min unit.
(8) When the G12.1/G13.1 command is issued, the deceleration check is executed.
(The coordinate commands in this interval will be the polar coordinate interpolation)
Plane selection
The linear axis and rotary axis used for polar coordinate interpolation must be set beforehand with
parameters.
(1) Determine the deemed plane for carrying out polar coordinate interpolation with the parameter (#1533) of
the linear axis used for polar 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)
(2) A program error (P485) will occur if the plane selection command (G16 to G19) is issued during the polar
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 when the parameter (#1533) is blank (no setting).
Related parameters
#1516 mill_ax (Milling axis name)
#1517 mill_c (Milling interpolation hypothetical axis name)
#8111 Milling Radius
#1533 millPax (Pole coordinate linear axis name)
76
Page 93
M700V/M70V Series Programming Manual (Machining Center System)
6.10 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113
Program example
N04
N05
N06
N07
N08
N09
N10
N01
N02
N11
N03
C
X
Hypothetical C axis
Hypothetical C axis
X
C
Z
Tool
Path after tool radius compensation
Program path
<Program>
:
:
N00 T0101;
:
:
N01 G17 G90 G0 X40.0 C0 Z0; Setting of start position
N02 G12.1; Polar coordinate interpolation mode: Start
N03 G1 G42 X20.0 F2000; Actual machining start
N04 C10.0;
N05 G3 X10.0 C20.0 R10.0;
N06 G1 X-20.0; Shape program
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; Polar coordinate interpolation mode: Cancel
:
:
M30 ;
(Follows orthogonal coordinate values on X-C hypothetical axis plane.)
77
Page 94
6 Interpolation Functions
MITSUBISHI CNC
Relation with other functions
Program commands during polar coordinate interpolation
(1) The program commands in the polar coordinate interpolation mode are issued by the orthogonal
coordinate value of the linear axis and rotary axis (hypothetical axis) on the polar coordinate interpolation
plane.
The axis address of the rotary axis (C) is specified as the axis address for the plane's 2nd axis
(hypothetical axis) command.
The command unit is not deg (degree). The same unit (mm or inch) as used for the command by the axis
address of the plane's 1st axis (linear axis) will be used.
(2) 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 polar coordinate
interpolation will start.
Circular interpolation on polar coordinate plane
The arc radius address for carrying out circular interpolation during the polar coordinate interpolation mode is
determined with the linear axis parameter (#1533).
#1533 setting value Center designation command
X I, J (polar coordinate plane is interpreted as XY plane)
Y J, K (polar coordinate plane is interpreted as YZ plane)
Z K, I (polar coordinate plane is interpreted as ZX plane)
Blank (no setting) I, J (polar 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 when the parameter (#1533) is blank (no setting).
Tool radius compensation
The tool radius can be compensated during the cylindrical interpolation mode.
(1) Command the plane selection in the same manner as polar coordinate interpolation.
When conducting tool radius compensation, it must be started up and canceled during the polar
coordinate interpolation mode.
(2) A program error (P485) will occur if polar coordinate interpolation is executed during tool radius
compensation.
(3) If the G12.1 and G13.1 commands are issued with no movement command 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.
Cutting asynchronous feed
(1) The asynchronous mode is forcibly set when the polar coordinate interpolation mode is started.
(2) When the polar coordinate interpolation mode is canceled, the synchronous mode will return to the state
before the polar coordinate interpolation mode was started.
(3) A program error (P485) will occur if G12.1 is commanded in the constant surface speed control mode
(G96).
78
Page 95
M700V/M70V Series Programming Manual (Machining Center System)
6.10 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113
Miscellaneous functions
(1) The miscellaneous function (M) and 2nd miscellaneous function can be issued in the polar coordinate
interpolation mode.
(2) The S command in the polar coordinate interpolation mode specifies the rotary tool's rotation speed
instead of the spindle rotation speed.
Tool length compensation
(1) Program error (P481) will occur if tool length compensation is performed 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 compensat ion in polar coordinate interpolation mode -> Program error
:
G13.1;
(2) 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 occur:
- Machine coordinate will not change even if G12.1 is executed.
- When G12.1 is executed, the workpiece coordinate will change to that of the post tool length
compensation.
(Even if the polar coordinate interpolation is canceled, this workpiece coordinate will not be canceled. )
F command during polar coordinate interpolation
As for the F command during polar coordinate interpolation mode, whether to use the previous F command
depends on the previous mode of the feed per minute command (G94/G98) or feed per rotation command
(G95/G99).
(1) When G94 (G98) is commanded just before G12.1
If there is no F command in the polar coordinate interpolation, the previous F command feedrate will be
used.
After the polar coordinate interpolation mode is canceled, the F command feedrate set at the start of the
polar coordinate interpolation mode or the last F command feedrate set during polar coordinate
interpolation will continue to be the feedrate.
(2) When G95 (G99) is commanded just before G12.1
The previous F command feedrate cannot be used during polar coordinate interpolation. A new F
command must be issued.
The feedrate after the polar coordinate interpolation mode is canceled will return to the state before the
polar coordinate interpolation mode was started.
[When there is no F command in G12.1]
Previous mode No F command After G13.1
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 With F command After G13.1
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.
79
Page 96
6 Interpolation Functions
MITSUBISHI CNC
Hole drilling axis in the fixed cycle for drilling command
Hole drilling axis in the fixed cycle for drilling command during the polar coordinate interpolation is determined
with the linear axis parameter (# 1533).
#1533 setting value Hole drilling axis
X Z (polar coordinate plane is interpreted as XY plane)
Y X (polar coordinate plane is interpreted as YZ plane)
Z Y (polar coordinate plane is interpreted as ZX plane)
Blank (no setting) Z (polar coordinate plane is interpreted as XY plane)
Shift amount in the G76 (fine boring) or G87 (back boring) command
Shift amount in the G76 (fine boring) or G87 (back boring) command during the polar coordinate interpolation
is determined with the linear axis parameter (#1533).
#1533 setting value Center designation command
X I, J (polar coordinate plane is interpreted as XY plane)
Y J, K (polar coordinate plane is interpreted as YZ plane)
Z K, I (polar coordinate plane is interpreted as ZX plane)
Blank (no setting) I, J (polar coordinate plane is interpreted as XY plane)
80
Page 97
M700V/M70V Series Programming Manual (Machining Center System)
6.10 Polar Coordinate Interpolation ; G12.1,G13.1/G112,G113
Restrictions and precautions
(1) The following G code commands can be used during the polar coordinate interpolation mode.
G code Details
G00 Positioning
G01 Linear interpolation
G02 Circular interpolation (CW)
G03 Circular interpolation (CWW)
G04 Dwell
G09 Exact stop check
G40-42 Tool radius compensation
G61 Exact stop mode
G64 Cutting mode
G65 Macro call (simple call)
G66 Macro modal call (modal call)
G66.1 Macro modal call (block call per macro)
G67 Macro modal call cancel (modal call cancel)
G80-89 Fixed cycle for drilling
G90/91 Absolute/incremental value command
G94 Asynchronous feed
G98 Hole drilling cycle initial return
G99 Hole drilling cycle R point return
A program error (P481) may occur if a G code other than those listed above is commanded during polar
coordinate interpolation.
(2) Program cannot be restarted (program restart) when the block is in the cylindrical interpolation.
(3) Before commanding polar coordinate interpolation, set the workpiece coordinate system so that the
center of the rotary axis is at the coordinate system zero point. Do not change the coordinate system
during the polar coordinate interpolation mode. (G50, G52, G53, relative coordinate reset, G54 to G59,
etc.)
(4) The feedrate during polar coordinate interpolation will be the interpolation speed on the polar coordinate
interpolation plane (orthogonal coordinate system).
(The relative speed with the tool will vary according to the polar coordinate conversion.)
When passing near the center of the rotary axis on the polar coordinate interpolation plane (orthogonal
coordinate system), the rotary axis side feedrate after polar coordinate interpolation will be very high.
(5) The axis movement command outside of the plane during polar coordinate interpolation will move
unrelated to the polar coordinate interpolation.
(6) The current position displays during polar coordinate interpolation will all indicate the actual coordinate
value. However, the "remaining movement amount" indicates the movement amount on the polar
coordinate input plane.
(7) The polar coordinate interpolation mode is canceled when the power is turned ON or reset.
(8) A program error (P484) will occur if any axis commanded during polar coordinate interpolation has not
completed the reference position return.
(9) Tool radius compensation must be canceled before canceling the polar coordinate interpolation mode.
(10) When the polar coordinate interpolation mode is canceled and switched to the cutting mode, the plane
selected before the polar coordinate interpolation will be restored.
(11) A program error (P486) will occur if the polar coordinate interpolation command is issued during the
mirror image.
(12) A program error (P481) will occur if the cylindrical interpolation or the polar coordinate interpolation is
commanded during the polar coordinate interpolation mode.
(13) During polar coor dinate interp olation, 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 minus
area that does not include "0" before issuing the polar coordinate interpolation command.
81
Page 98
6 Interpolation Functions
MITSUBISHI CNC
6.11 Exponential Interpolation ; G02.3,G03.3
J1 J2
J3
(G02.3/G03.3)
(G00)
(G01)
(G01)
A
Z
X
A
Function and purpose
Exponential function interpolation changes the rotary 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
A : A axis (rotary axis)
X : X axis (linear axis)
Torsion angle : J1 = J2 = J3
- Relation of linear axis and rotary axis
X
X=B(eCA-1)
*
A : A axis (rotary axis)
X : X axis (linear axis)
* : {B, C... constant}
82
Page 99
M700V/M70V Series Programming Manual (Machining Center System)
6.11 Exponential Interpolation ; G02.3,G03.3
Command format
G02.3 Xx1 Yy1 Zz1 Ii1 Jj1 Rr1 Ff1 Qq1 Kk1 ; ... Forward rotation interpolation (modal)
G03.3 Xx1 Yy1 Zz1 Ii1 Jj1 Rr1 Ff1 Qq1 Kk1 ; ... 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 specified by parameter "#1514 expLinax" and the axis that
carries out linear interpolation between that axis.
If the end point on of the rotary axis designated with parameter "#1515 expRotax" is specified,
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 per
minute feed. )
Command the composite feedrate that includes the rotary 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.
(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 rotary 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.
83
Page 100
6 Interpolation Functions
MITSUBISHI CNC
- Example of uniform helix machining of taper shape
i1
j1
x1x0
r1
ZZ
A
X
A : A axis (rotary axis) X : X axis (linear axis) x0 : linear axis start point
Detailed description
Relational expression of exponential function
The exponential function relational expression of the linear axis (X) and rotary axis (A) in the G02.3/G03.3
command is defined in the following manner.
θ/D
X(θ) = r1 * (e
- 1) / tan(i1) ...(linear axis (X) movement (1))
A(θ) = (-1)ω * 360 * θ / (2π) ...(rotary axis (A) movement)
However,
D = tan (j1) / tan (i1)
ω = 0 during forward rotation (G02.3), and ω = 1 during reverse rotation (G03.3).
θ is the rotation angle (radian) from the rotary axis' start point
The rotary axis' rotation angle (θ) is as follows according to expression (1).
θ = D * 1n｛(X * tan(i1) / r1) + 1｝
84
Loading...