MITSUBISHI CNC M700L, M700LV, M70L Programming Manual
MELDAS is a registered trademark of Mitsubishi Electric Corporation.
Other brands and product names throughout this manual are trademarks or registered
trademarks of their respective holders.
Introduction
This instruction manual describes the methods of using the MITSUBISHI CNC
MULTI-AXIS,MULTI-PART SYSTEM M700L/M700LV/M70L Series mainly for a lathe.
The programming methods for all of the above models are described, so read this manual
thoroughly before starting use.
In respect to the functions related to the multi-axis multi-part system, the programming and
alarm details for each system are the same as the general-purpose (2-axis, 3-axis) lathe.
Explanations in this manual assume that all functions are provided with all of the above
models. However, all options are not necessarily provided with each CNC, so refer to the
specifications issued by the machine manufacturer before starting use.
Thoroughly read the "Precautions for Safety" given on the next page to ensure safe use of
this numerical control unit.
Details described in this manual
(1) This manual gives general explanations from the standpoint of the NC side.
For explanations concerning individual machine tools, refer to the instruction manual
issued by the machine manufacturer.
For items described as "Restrictions, "Usable State", etc., the instruction manual issued by
the machine manufacturer takes precedence over this manual.
(2) While every effort has been made to describe special handling in this manual, items not
described in this manual should be interpreted as "Not Possible".
(3) The multi-part system function is an additional specification. The 3-system model is
explained as an example in this manual, but the number of systems that can be used will
differ according to the model.
Note that the maximum number of spindle axes will also differ according to the model.
Check the specifications before starting use.
(4) Some functions are unavailable depending on the machine model.
CAUTION
For items described in "Restrictions" or "Usable State", the instruction manual issued by the
machine manufacturer takes precedence over this manual.
Items not described in this instruction manual should be interpreted as "Not Possible".
This manual has been writt en on t h e a s s u mptio n t h a t all op t i o n f u n c t ions a r e added.
Refer to the specifications issued by the machine manufacturer before starting use.
Refer to the instruction manual issued by the machine manufacturer for explanations on each
machine tool.
Some screens and functions may differ or may not be usable depending on the NC system
version.
Precautions for Safety
Always read the specifications issued by the machine maker, this manual, related manuals
and attached documents before installation, operation, programming, maintenance or
inspection to ensure correct use.
Understand this numerical controller, safety items and cautions before using the unit.
This manual ranks the safety precautions into "DANGER", "WARNING" and "CAUTION".
DANGER
WARNING
CAUTION
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
Not applicable in this manual.
CAUTION
1. Items related to product and manual
For items described as "Restrictions" or "Usable State" in this manual, the instruction manual
issued by the machine manufacturer takes precedence over this manual.
Items not described in this instruction manual should be interpreted as "Not Possible".
This manual is written on the assumption that all option functions are added. Refer to the
specifications issued by the machine manufacturer before starting use.
Some screens and functions may differ or may not be usable depending on the NC system
version.
CAUTION
2. Items related to programming
Because of key chattering etc., during editing, the commands with no value after G become a
"G00" operation during running.
";", "EOB" and "%" "EOR" are expressions used for the explanation. The actual codes are
"; (line feed)" and "%" for ISO, and "EOB" (End Of Block) and "EOR" (End Of Record) for
EIA.
The commands with no value after G become a "G00" operation during running.
Always carry out dry run operation before actual machining, and confirm the machining
program, tool offset amount and workpiece offset amount, etc.
When creating the machining program, select adequate machining conditions, and make
sure not to exceed the machine and NC's performance, capacity and limits. Examples
given in this manual do not take the machining conditions into consideration.
Do not change fixed cycle programs without the prior approval of the machine
manufacturer.
When programming the multi-part system, take special care to the movements of the
programs for other systems.
During the spindle synchronous control mode, do not turn the rotation command for the
slave spindle OFF while the master spindle and slave spindle are chucked on the same
workpiece. This will be hazardous as the slave spindle will stop.
Do not issue another axis name change command before axis name change cancel is
issued once axis name change is commanded.
Disposal
(Note) This symbol mark is for EU countries only.
This symbol mark is according to the directive 2006/66/EC Article 20 Information for endusers and Annex II.
Your MITSUBISHI ELECTRIC product is designed and manufactured with high quality materials and
components which can be recycled and/or reused.
This symbol means that batteries and accumulators, at their end-of-life, should be disposed of
separately from your household waste.
If a chemical symbol is printed beneath the symbol shown above, this chemical symbol means that the
battery or accumulator contains a heavy metal at a certain concentration. This will be indicated as
follows:
Hg: mercury (0,0005%), Cd: cadmium (0,002%), Pb: lead (0,004%)
In the European Union there are separate collection systems for used batteries and accumulators.
Please, dispose of batteries and accumulators correctly at your local community waste collection/
recycling centre.
Please, help us to conserve the environment we live in!
Contents
1. CONTROL AXES............................................................................................................................1
1.1 Coordinate Word and Control Axis..........................................................................................1
1.2 Coordinate Systems and Coordinate Zero Point Symbols......................................................2
2. INPUT COMMAND UNITS .............................................................................................................3
2.1 Input Command Units .............................................................................................................3
2.2 Input Setting Units...................................................................................................................3
3. DATA FORMATS ...........................................................................................................................4
3.1 Tape Codes.............................................................................................................................4
3.2 Program Formats ....................................................................................................................6
3.3 Tape Storage Format..............................................................................................................8
3.4 Optional Block Skip.................................................................................................................8
3.5 Program/Sequence/Block Numbers (O, N).............................................................................9
3.6 G Code System.....................................................................................................................10
3.7 Precautions Before Machining ..............................................................................................14
4. BUFFER REGISTER....................................................................................................................15
4.1 Pre-read Buffers....................................................................................................................15
5. POSITION COMMANDS ..............................................................................................................16
5.1 Incremental/Absolute Value Commands...............................................................................16
5.2 Radius/Diameter Commands ................................................................................................18
5.3 Inch/Metric Conversion (G20, G21) ......................................................................................19
5.4 Decimal Point Input...............................................................................................................20
6. INTERPOLATION FUNCTIONS...................................................................................................24
6.1 Positioning (Rapid Traverse); G00........................................................................................24
6.2 Linear Interpolation; G01.......................................................................................................27
6.3 Circular Interpolation; G02, G03 ...........................................................................................29
6.4 R-designated Circular Interpolation; G02, G03.....................................................................33
6.5 Plane Selection; G17, G18, G19...........................................................................................35
6.6 Helical interpolation; G17, G18, G19, and G02, G03............................................................37
6.7 Thread Cutting ......................................................................................................................41
6.7.1 Constant lead thread cutting; G33..................................................................................41
6.7.2 Inch thread cutting; G33 .................................................................................................45
6.7.3 Continuous thread cutting...............................................................................................46
6.7.4 Variable lead thread cutting............................................................................................47
6.7.5 Circular thread cutting; G35/G36....................................................................................49
6.8 Milling Interpolation; G12.1/G13.1.........................................................................................55
6.8.1 Selecting milling mode....................................................................................................56
6.8.2 Milling interpolation control and command axes.............................................................57
6.8.3 Selecting a plane during the milling mode......................................................................59
6.8.4 Setting milling coordinate system ...................................................................................61
6.8.5 Preparatory functions......................................................................................................63
6.8.6 Switching from milling mode to turning mode; G13.1 .....................................................68
6.8.7 Feed function ..................................................................................................................68
6.8.8 Program support functions..............................................................................................68
6.8.9 Miscellaneous functions..................................................................................................69
6.8.10 Tool offset functions......................................................................................................70
6.8.11 Interference check ........................................................................................................87
7. FEED FUNCTIONS.......................................................................................................................95
7.1 Rapid Traverse Rate.............................................................................................................95
7.2 Cutting Feedrate ...................................................................................................................95
7.3 Synchronous/Asynchronous Feed; G94, G95.......................................................................96
7.4 Feedrate Designation and Effects on Control Axes ..............................................................98
7.5 Thread Cutting Leads..........................................................................................................102
7.6 Automatic Acceleration/Deceleration ..................................................................................103
7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration.........................................104
7.8 Speed Clamp ......................................................................................................................106
7.9 Exact Stop Check; G09.......................................................................................................107
7.10 Exact Stop Check Mode; G61...........................................................................................111
7.11 Cutting Mode; G64............................................................................................................111
7.12 Feed Forward Control .......................................................................................................112
8. DWELL .......................................................................................................................................113
8.1 Dwell Per Second; (G94) G04.............................................................................................113
8.2 Dwell Per Rotation; (G95) G04 ...........................................................................................115
9. MISCELLANEOUS FUNCTIONS...............................................................................................116
9.1 Miscellaneous Functions (M2-digit BCD)............................................................................116
9.2 Miscellaneous Functions (M8-digit).....................................................................................118
9.3 2nd Miscellaneous Functions (A8/B8/C8-digit) ...................................................................118
10. SPINDLE FUNCTIONS.............................................................................................................119
10.1 Spindle Functions (S2-digit BCD) .....................................................................................119
10.2 Spindle Functions (S8-digit)..............................................................................................119
10.3 Constant Surface Speed Control; G96, G97.....................................................................120
10.4 Spindle Clamp Speed Setting; G92 ..................................................................................127
10.5 Spindle Functions (Multiple Spindles)...............................................................................129
10.5.1 Multiple-spindle commands ........................................................................................130
10.6 Second Spindle Control Function......................................................................................132
10.6.1 Second spindle extension selection............................................................................134
11. TOOL FUNCTIONS..................................................................................................................135
11.1 Tool Functions (T4-digit) ...................................................................................................135
11.2 Tool Functions (T8-digit) ...................................................................................................136
11.3 Number of T Command Digits Judgment Function...........................................................137
12. TOOL OFFSET FUNCTIONS...................................................................................................139
12.1 Tool Offset.........................................................................................................................139
12.2 Tool Length Offset.............................................................................................................141
12.3 Tool Nose Wear Offset......................................................................................................143
12.3.1 Wear offset amount hold.............................................................................................144
12.4 Nose R Compensation; G40, G41, G42, G46...................................................................145
12.4.1 Tool nose point and compensation directions ............................................................147
12.4.2 Nose R compensation operations...............................................................................150
12.4.3 Other operations during nose R compensation ..........................................................160
12.4.4 G41/G42 commands and I, J, K designation..............................................................168
12.4.5 Interrupts during nose R compensation......................................................................173
12.4.6 General precautions for nose R compensation...........................................................176
12.4.7 Interference check ......................................................................................................177
12.5 Programmed Tool Offset Input; G10.................................................................................182
12.6 Common System Offset....................................................................................................185
13. PROGRAM SUPPORT FUNCTIONS.......................................................................................186
13.1 Fixed Cycles for Turning ...................................................................................................186
13.1.1 Longitudinal cutting cycle; G77...................................................................................187
13.1.2 Thread cutting cycle; G78...........................................................................................189
13.1.3 Face cutting cycle; G79 ..............................................................................................192
13.2 Compound Fixed Cycles...................................................................................................195
13.2.1 Longitudinal rough cutting cycle I; G71.......................................................................196
13.2.2 Face rough cutting cycle I; G72..................................................................................201
13.2.3 Formed material rough cutting cycle; G73..................................................................206
13.2.4 Finishing cycle; G70 ...................................................................................................210
13.2.5 Face cut-off cycle; G74...............................................................................................211
13.2.6 Longitudinal cut-off cycle; G75 ...................................................................................213
13.2.7 Compound thread cutting cycle; G76..........................................................................215
13.2.8 Precautions for compound fixed cycles (G70 to G76) ................................................219
13.3 Hole Drilling Fixed Cycles; G80 to G89.............................................................................221
13.3.1 G83 face deep hole drilling cycle 1 (G87 longitudinal deep hole drilling cycle 1).......225
13.3.2 G84 face tapping cycle (G88 longitudinal tapping cycle)............................................227
13.3.3 G85 face boring cycle (G89 longitudinal boring cycle)................................................232
13.3.4 G80 hole drilling fixed cycle cancel.............................................................................232
13.3.5 Precautions for using hole drilling fixed cycles ...........................................................233
13.4 Deep Hole Drilling Cycle 2; G83.2 ....................................................................................234
13.5 Subprogram Control; M98, M99........................................................................................237
13.6 Variable Commands..........................................................................................................243
13.7 User Macro........................................................................................................................245
13.7.1 User macro commands; G65, G66, G66.1, G67.........................................................245
13.7.2 Macro call instruction..................................................................................................246
13.7.3 G code for macro........................................................................................................253
13.7.4 Variables.....................................................................................................................254
13.7.5 Types of variables.......................................................................................................256
13.7.6 Operation commands..................................................................................................271
13.7.7 Control commands......................................................................................................276
13.7.8 Precautions.................................................................................................................279
13.8 Double-Turret Mirror Image; G68, G69.............................................................................281
13.9 Corner Chamfering, Corner Rounding Function I .............................................................286
13.9.1 Corner chamfering (,C_ )............................................................................................286
13.9.2 Corner rounding (,R_ )................................................................................................288
13.10 Corner Chamfering, Corner Rounding Function II ..........................................................290
13.10.1 Corner chamfering (,C_) ...........................................................................................290
13.10.2 Corner rounding (,R_ )..............................................................................................292
13.10.3 Interrupt during corner chamfering/rounding.............................................................294
13.11 Linear Angle Command ..................................................................................................295
13.12 Geometric Command ......................................................................................................296
13.12.1 Geometric command IA ............................................................................................296
13.13 Program Parameter Input; G10/G11...............................................................................299
13.14 Programmable In-position Check....................................................................................307
13.15 Positioning (G00)/Machine Coordinate System Selection (G53) Feedrate
Designation.....................................................................................................................310
13.16 Inclined Coordinate Rotation; G173................................................................................316
14. COORDINATE SYSTEM SETTING FUNCTIONS....................................................................328
14.1 Coordinate Words and Control Axes.................................................................................328
14.2 Basic Machine, Workpiece and Local Coordinate Systems..............................................329
14.3 Machine Zero Point and 2nd Reference Point (Zero Point) ..............................................330
14.4 Automatic Coordinate System Setting ..............................................................................331
14.5 Machine Coordinate System Selection; G53 ....................................................................332
14.6 Coordinate System Setting; G92.......................................................................................333
14.7 Reference Point Return; G28, G29...................................................................................334
14.8 2nd, 3rd, and 4th Reference (Zero) Point Return; G30.....................................................338
14.9 Reference Point Check; G27 ............................................................................................341
14.10 Workpiece Coordinate System Setting and Offset; G54 to G59 .....................................342
14.11 Local Coordinate System Setting; G52...........................................................................347
15. PROTECTION FUNCTIONS.....................................................................................................348
15.1 Chuck Barriers/Tailstock Barriers......................................................................................348
16. MEASUREMENT SUPPORT FUNCTIONS..............................................................................351
16.1 Skip Function; G31............................................................................................................351
16.2 Multi-step Skip Function; G31...........................................................................................356
16.3 Automatic Tool Length Measurement; G37 ......................................................................358
17. MULTI-AXIS, MULTI-PART SYSTEM COMPOUND CONTROL FUNCTIONS.......................361
17.1 Synchronizing Operation between Systems .....................................................................364
17.2 Start Point Designation Synchronizing (Type 1); G115.....................................................369
17.3 Start Point Designation Synchronizing (Type 2); G116.....................................................371
17.4 Balance Cut Command; G15, G14 ...................................................................................373
17.5 Program Call Control.........................................................................................................376
17.6 Cross Axis Control; G110..................................................................................................377
17.7 Control Axis Synchronization ; G125 ................................................................................383
17.8 Spindle Synchronization; G114.1, G113...........................................................................386
17.9 Tool/Spindle Synchronization 1 (Polygon); G114.2, G113................................................393
17.10 Tool/Spindle Synchronization 2 (Hobb Machining); G114.3, G113.................................400
17.11 Control Axis Superimposition; G126 ...............................................................................411
17.12 Spindle Superimposition; G164, G113............................................................................426
17.12.1 Relation with other functions.....................................................................................430
17.12.2 Precautions and restrictions .....................................................................................431
17.13 2-System Simultaneous Thread-cutting Cycle................................................................433
17.13.1 Parameter setting command.....................................................................................433
17.13.2 2-system simultaneous thread-cutting cycle I...........................................................434
17.13.3 2-system simultaneous thread cutting cycle II..........................................................436
18. OTHER MULTI-AXIS, MULTI-PART SYSTEM CONTROL FUNCTIONS................................439
18.1 Miscellaneous Function Output during Axis Movement; G117 .........................................439
18.2 G Code Macros.................................................................................................................441
18.3 Axis Name Change; G111 ................................................................................................442
APPENDIX 1 LIST OF FUNCTION CODES................................................................................450
APPENDIX 2 LIST OF COMMAND VALUES AND SETTING RANGES....................................451
APPENDIX 3 CIRCULAR CUTTING RADIUS ERROR...............................................................452
APPENDIX 4 STANDARD FIXED CYCLE SUBPROGRAMS.....................................................453
APPENDIX 5 LIST OF VARIABLE NUMBERS...........................................................................461
APPENDIX 6 CORRESPONDENCE TABLE OF PROGRAM PARAMETER INPUT N NUMBERS
...............................................................................................................................463
6.1.1 Control parameter.........................................................................................................464
6.1.2 Axis parameter..............................................................................................................466
6.1.3 Setup parameter ...........................................................................................................467
6.1.4 Setup parameter 2 ........................................................................................................469
6.2.1 Base axis parameter.....................................................................................................470
6.2.2 Base system parameter................................................................................................471
6.2.3 Base common parameter..............................................................................................473
6.2.4 Axis specification parameter.........................................................................................475
6.2.5 Zero point return parameter..........................................................................................476
6.2.6 Absolute position set.....................................................................................................477
6.2.7 Position switch ..............................................................................................................477
6.2.8 Servo parameter ...........................................................................................................478
6.2.9 Machine error compensation ........................................................................................478
6.2.10 Machine compensation data.......................................................................................478
6.2.11 Macro list ....................................................................................................................479
6.2.12 Spindle NC parameter ................................................................................................484
6.2.13 Spindle parameter.......................................................................................................485
6.2.14 Spindle type servo parameter.....................................................................................485
6.2.15 PLC constant ..............................................................................................................486
6.2.16 PLC timer....................................................................................................................486
6.2.17 PLC counter................................................................................................................486
6.2.18 Bit selection ................................................................................................................486
APPENDIX 7 SUPPLEMENTARY DETAILS ON INCOMPLETE THREAD AREAS ARISING
DURING THREAD CUTTING................................................................................487
APPENDIX 8 MACRO INTERFACE EXPANSION......................................................................491
8.1 Macro Interface Input ..........................................................................................................492
8.2 Macro Interface Output .......................................................................................................494
APPENDIX 9 SYSTEM COMMON POSITION INFORMATION RETRIEVING VARIABLES......496
APPENDIX 10 PROGRAM ERRORS..........................................................................................498
1. CONTROL AXES
p
r
r
1. CONTROL AXES
1.1 Coordinate Word and Control Axis
Function and purpose
In the case of a lathe, the axis parallel to the spindle is known as the Z axis and its forward
direction is the direction in which the turret moves away from the spindle stock while the axis at
right angles to the Z axis is the X axis and its forward direction is the direction in which it moves
away from the Z axis, as shown in the figure below.
1.1 Coordinate Word and Control Axis
indle stock
S
+Y
Tailstock
Tool
Tu
et
+Z
+X
Coordinate axes and polarities
Since coordinates based on the right hand rule are used with a lathe, the forward direction of the
Y axis in the above figure which is at right angles to the X-Z plane is downward. It should be
borne in mind that an arc on the X-Z plane is expressed as clockwise or counterclockwise as
seen from the forward direction of the Y axis. (Refer to the section on circular interpolation.)
Spindle nose
Machine zero point
G54
G55
G58
G52
Workpiece zero points (G54 to G59)
G59
Local coordinate system
(Valid in G54 to G59)
G30
2nd reference position
+Z
G28
+X
Reference position
(+Y)
Relationship between coordinates
1
1. CONTROL AXES
X
X
X
X
1.2 Coordinate Systems and Coordinate Zero Point Symbols
1.2 Coordinate Systems and Coordinate Zero Point Symbols
Function and purpose
: Reference position
: Machine coordinate origin
: Workpiece coordinate zero points
(G54 to G59)
Upon completion of the reference point return, the parameters are referred to and automatically
set for the basic machine coordinate system and workpiece coordinate systems (G54 to G59).
The basic machine coordinate system is set so that the first reference point is at the position
designated by the parameter from the basic machine coordinate zero point (machine zero point).
Basic mac hine
coordinate system
Hypothetical machine
coordinate system
(shifted by G92)
+
2
Z2
Machine zero point
Workpiece
coordinate
system
1 (G54)
Workpiece
coordinate
system
2 (G55)
+Z
Workpiece
coordinate
system
5 (G58)
Workpiece
coordinate
system6
(G59) Z
3
Z
3
Local
coordinate
system
1
(G52)
1
1st reference position
The local coordinate system (G52) is valid on the coordinate systems designated by the
commands for the workpiece coordinate systems 1 to 6.
Using the G92 command, the basic machine coordinate system can be shifted and made the
hypothetical machine coordinate system. At the same time, workpiece coordinate systems 1 to 6
are also shifted.
2
2. INPUT COMMAND UNITS
2. INPUT COMMAND UNITS
2.1 Input Command Units
2.2 Input Setting Units
Function and purpose
These are the units used for the movement amounts in the program as commanded by the MDI
input. They are expressed in millimeters, inches or degrees (°).
Function and purpose
These are the units of setting data which are used, as with the compensation amounts, in
common for all axes.
The input command unit can be selected for each axis and input setting units can be selected in
common for the axes by parameters from among the following types. (For further details on
settings, refer to the sections about control.)
Type
Input
command unit
Min. movement
unit
Input setting
unit
(Note 1) Inch/metric conversion is performed in either of 2 ways: conversion from the Parameter
screen ("Initial inch": valid only when the power is turned ON) and conversion using the
G command (G20 or G21).
However, when a G command is used for the conversion, the conversion applies only to
the input command units and not to the input setting units.
Consequently, the tool offset amounts and other compensation amounts as well as the
variable data should be preset to correspond to input setting unit.
#1003
cunit=10
=1 0.0001 0.0001 0.00001 0.00001 0.0001
IS-B 0.0005 0.001 0.0005 0.0001 0.001
IS-C 0.00005 0.0001 0.00005 0.00001 0.0001
IS-B 0.001 0.001 0.0001 0.0001 0.001
IS-C 0.0001 0.0001 0.00001 0.00001 0.0001
2.1 Input Command Units
Linear axis
Millimeter Inch
Diametrical
command
0.001 0.001 0.0001 0.0001 0.001
Radial
command
Diametrical
command
Radial
command
Rotation
axis
(°)
(Note 2) The millimeter and inch systems cannot be used together.
3
3. DATA FORMATS
3. DATA FORMATS
3.1 Tape Codes
Function and purpose
The tape command codes used for this NC are combinations of alphabet letters (A, B, C...Z),
numbers (0, 1, 2...9) and signs ( +, –, /...). These alphabet letters, numbers and signs are referred
to as characters. Each character is represented by a combination of 8 holes which may, or may
not, be present.
These combinations make up what is called codes.
This NC employs the ISO code (R-840).
CAUTION
";", "EOB" and "%" "EOR" are expressions used for the explanation. The actual codes are "line
feed" and "%" for ISO.
Detailed description
(1) For the sake of convenience, a ";" has been used in the NC display to indicate End Of Block
(EOB/LF) which separates one block from another. Do not use the ";" key, however, in actual
programming but use the keys in the following table instead.
EOB/EOR keys and displays
3.1 Tape Codes
Code used
Key used
End Of Block LF or NL ;
End Of Record % %
(Note 1) If a code not given in Table of tape codes is assigned during operation, an Illegal
address error "P32" will result.
(Note 2) The following codes which exist with ISO can be designated by parameter:
[ (left square parenthesis)
] (right square parenthesis)
# (sharp sign)
∗ (asterisk)
= (equals sign)
: (colon)
! (exclamation mark) = (queuing code)
$ (dollar sign) = (code designating system number)
Any codes which overlap with existing codes or codes which result in parity H cannot be
designated.
ISO NC display
4
3. DATA FORMATS
G
R
•
•••••••
•
•••
•
• •
•
•••••••••
•
•••••••
•
•
•••••••••••••••••
•
•
•
•••••••••••••••
•
•
•••••••••
(2) Significant data section (label skip function)
(3) Control out, control in
3.1 Tape Codes
All data up to the first EOB (;), after the power has been turned ON or after operation has
been reset, are ignored during automatic operation based on tape, memory loading
operation or during a search operation. In other words, the significant data section of a tape
extends from the character or number code after the first EOB (;) code after resetting to the
point where the reset command is issued.
When the ISO code is used, all data between control out "(" and control in ")" are ignored by
the NC, although these data appear on the setting display unit. Consequently, the command
tape name, number and other such data not directly related to control can be inserted in this
section.
This information will also be loaded, however, during tape loading.
The system is set to the "control in" mode when the power is turned ON.
Example of ISO code
••
• • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • •
•• •••
•
•• •••
•
•
•
Operator information print-out example
L C S L
00X-85000Y-64000 (CUTTE
F R
• •
•• ••
••
•
• •• •
Information in this section is ignored and nothing is executed.
RE T URN)
P
• • •
• •• •
••• • ••
•••
•
•
••••••
••• • • •
F
••
•••••
•
(4) EOR (%) code
Generally, End Of Record is punched at both ends of the tape. It has the following functions:
(a) Rewind stop when rewinding tape (with tape handler)
(b) Rewind start during tape search (with tape handler)
(c) Completion of loading during tape loading
5
3. DATA FORMATS
3.2 Program Formats
Function and purpose
The prescribed arrangement used when assigning control information to the NC unit is known as
the "program format", and the format used with the NC is called the "word address format."
Detailed description
(1) Word and address
A word is a collection of characters arranged in a specific sequence. This entity is used as
the unit for processing data and for causing the NC to execute specific operations.
Each word used for the NC consists of an alphabet letter and a number of several digits
(sometimes with a "+" or "–" sign placed at the head of the number).
Word
Numerical (word data)
Alphabet (address)
3.2 Program Formats
------
Word configuration
The alphabet letter at the head of the word is the address. It defines the meaning of the
numerical information which follows it.
With the NC, "S
=" can be commanded for a multiple number of spindle commands
although this applies only to address S.
For details of the types of words and the number of significant digits of numbers used for this
NC, refer to Table 1 Format details and abbreviations.
(2) Blocks
A block is a collection of words. It includes the information which is required for the NC to
execute one specific operation. One block unit constitutes a complete command. The end of
each block is marked with an EOB (End-Of-Block) code.
(3) Programs
A program is a collection of several blocks.
(Note 1) If there is no number after the alphabetic character in the actual program, the value
following the alphabetic character will be handled as 0.
(Example) G28XYZ; → G28X0Y0Z0;
6
3. DATA FORMATS
(Note 1) "
3.2 Program Formats
Table 1 Format details and abbreviations
Item Abbreviation
Program number O8
Sequence number N5
Preparatory function G3/G21
Movement
command
Movement
command, circular,
cutter radius
Dwell
Feed function
Input setting unit A 0.01°, mm
Input setting unit B 0.001°, mm
Input setting unit C 0.0001°, mm
Input setting unit A 0.01°, mm
Input setting unit B 0.001°, mm
Input setting unit C 0.0001°, mm
Input setting unit A 0.01°, mm
Input setting unit B 0.001°, mm
Input setting unit C 0.0001°, mm
Input setting unit A 0.01°, mm
X + 62 Z + 62
X + 53 Z + 53
X + 44 Z + 44
I + 62 K + 62
I + 53 K + 53
I + 44 K + 44
X + 53 P8
X + 53 P8
X + 53 P8
F62 (feed per minute)
+ 62
+ 53
+ 44
F43 (feed per rotation)
Input setting unit B 0.001°, mm
F53 (feed per minute)
F34 (feed per rotation)
Input setting unit C 0.0001°, mm
F54 (feed per minute)
F25 (feed per rotation)
Tool offset T1/T2
Miscellaneous function M2/M8
Spindle function S2/S5/S8 or S = n
Tool function T2/T8
2nd miscellaneous function A8/B8/C8
Subprogram P8H5L4
Fixed cycle
Input setting unit A 0.01°, mm
Input setting unit B 0.001°, mm
Input setting unit C 0.0001°, mm
R + 62 Q62 P8 L4
R + 53 Q53 P8 L4
R + 44 Q44 P8 L4
" denotes the A, B, C, Y, P or R.
(Note 2) The number of digits in the words is checked by the maximum number of digits in the
addresses.
7
3. DATA FORMATS
3.3 Tape Storage Format
Function and purpose
(1) Storage tape and storage sections
The section which is stored into the memory extends from the character following the head
EOB after resetting as far as the EOR code.
The significant codes listed in Table of tape codes in Section 3.1 are the codes in the above
storage section which are actually stored into the memory. All other codes are ignored and
are not stored.
The data between control out "(" and control in ")" are stored into the memory.
3.4 Optional Block Skip
Function and purpose
This function selectively ignores specific blocks in a machining program which starts with the "/"
(slash) code.
Detailed description
(1) Provided that the optional block skip switch is ON, blocks starting with the "/" code are
ignored. They are executed if the switch is OFF.
Parity check is valid regardless of whether the optional block skip switch is ON or OFF.
When, for instance, all blocks are to be executed for one workpiece but specific 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 for using optional block skip
(1) Put the "/" code at the head of the block. When inserted in a block, this is handled as a
division sign.
3.3 Tape Storage Format
(Example) N20G1X25./Z25.;............. NG
(This will be handled as 25. /0, so the error P283
"Divided by zero" will occur.)
/N20G1X25.Z25.;............. OK
(2) Parity checks (H and V) are conducted regardless of the optional block skip switch state.
(3) The optional block skip is processed immediately before the pre-read buffer.
Consequently, it is not possible to skip up to the block which has been read into the pre-read
buffer.
(4) This function is valid even during a sequence number search.
(5) AII blocks with the "/" code are also input and output during tape storing and tape output,
regardless of the state of the optional block skip switch.
8
3. DATA FORMATS
3.5 Program/Sequence/Block Numbers (O, N)
3.5 Program/Sequence/Block Numbers (O, N)
Function and purpose
These numbers are used for monitoring the execution of the machining programs and for calling
both machining programs and specific stages in machining programs.
(1) Program numbers are classified by workpiece correspondence or by subprogram units, and
they are designated by the address "O" followed by a number with up to 8 digits.
(2) Sequence numbers are attached where appropriate to command blocks which configure
machining programs, and they are designated by the address "N" followed by a number with
up to 5 digits.
(3) Block numbers are automatically provided inside the NC itself. They are preset to "0" every
time a program number or sequence number is read, and they are counted up one at a time
unless program numbers or sequence numbers are commanded in blocks which are
subsequently read.
Consequently, all the blocks of the machining programs given in the table below can be
determined without further consideration by combinations of program numbers, sequence
numbers and block numbers.
NC input machining program
O12345678 (DEMO.PROG); 12345678 0 0
N100 G00 G90 X120. Z100.; 12345678 100 0
G94 S1000; 12345678 100 1
N102 G71 P210 Q220 I0.2 K0.2 D0.5 F600; 12345678 102 0
N200 G94 S1200 F300; 12345678 200 0
N210 G01 X0 Z95.; 12345678 210 0
G01 X20.; 12345678 210 1
G03 X50. Z80. K–15.; 12345678 210 2
G01 Z55.; 12345678 210 3
G02 X80. Z40. I15.; 12345678 210 4
G01 X100.; 12345678 210 5
G01 Z30.; 12345678 210 6
G02 Z10. K–15.; 12345678 210 7
N220 G01 Z0; 12345678 220 0
N230 G00 X120. Z150.; 12345678 230 0
N240 M02; 12345678 240 0
% 12345678 240 0
Program
No.
NC monitor display
Sequence
No.
Block
No.
9
3. DATA FORMATS
3.6 G Code System
Function and purpose
These numbers are used to monitor the execution status of the machining program, or to call a
machining program or a specific process in the machining program.
There are 3 G code systems: 1, 2 and 3. Parameters "G code type 1", "G code type 2" and "G
code type 3" are used to set the applicable system.
G code system 3 is an additional specification.
The description of the G functions is based on G code system 2 which serves as the standard.
(Note 1) An alarm results when a G code not listed in the table is commanded. ("P34": Illegal G
code)
(Note 2) An alarm results when a G code not included in the additional specifications is
commanded.
(Example) An alarm ("P50 No spec: Inch/mm") occurs when the inch command G
3.6 G Code System
code (G20) is commanded although the inch/mm specifications have not
been provided.
Table of G code systems
Reference
G code system (standard = 2) Group Function name
1 2 3
G00 G00 G00 01 Positioning 6.1
G01 G01 G01 01 Linear interpolation 6.2
G02 G02 G02 01 Circular interpolation (clockwise) 6.3, 6.4
G03 G03 G03 01 Circular interpolation (counterclockwise) 6.3, 6.4
G04 G04 G04 00 Dwell 8.1, 8.2
G09 G09 G09 00 Exact stop 7.8
G10 G10 G10 00 Data setting 12.5
G11 G11 G11 00 Data setting mode cancel 12.1
G12.1 G12.1 G12.1 19 Milling mode ON 6.8
G13.1 G13.1 G13.1 19 Milling mode OFF
G14 G14 G14 18 Balance cut OFF 17.4
G15 G15 G15 18 Balance cut ON
G16
G17 G17 G17 02 X-Y plane selection 6.5
G18 G18 G18 02 Z-X plane selection
G19 G19 G19 02 Y-Z plane selection
G20 G20 G70 06 Inch command
G21 G21 G71 06 Metric command
G22 G22 G22 04 Barrier check ON 15.1
G23 G23 G23 04 Barrier check OFF
G16 G16 02 Y-Z cylindrical plane selection 6.8
section in this
manual
(Section)
5.3
10
3. DATA FORMATS
G code system (standard = 2) Group Function name
G27 G27 G27 00 Reference point return check 14.9
G28 G28 G28 00 Reference point return 14.7
G29 G29 G29 00 Return from reference point
G30 G30 G30 00 2nd reference point return 14.8
G31 G31 G31 00 Skip function 16.1
G32 G33 G33 01 Thread cutting 6.7
G34 G34 G34 01 Variable lead thread cutting
G35 G35 G35 01 Circular thread cutting (CW)
G36 G36 G36 01 Circular thread cutting (CCW)
G37 G37 G37 00
G40 G40 G40 07 Tool nose R compensation cancel 12.4
G41 G41 G41 07 Tool nose R compensation left
G42 G42 G42 07 Tool nose R compensation right
G43 G43 G43 08 2nd spindle control OFF 10.6
G44 G44 G44 08 2nd spindle control ON
G46 G46 G46 07
G50 G92 G92 00
G52 G52 G52 00 Local coordinate system setting 14.11
G53 G53 G53 00 Machine coordinate system selection 14.5
G54 G54 G54 12 Workpiece coordinate system selection 1 14.10
G55 G55 G55 12 Workpiece coordinate system selection 2
G56 G56 G56 12 Workpiece coordinate system selection 3
G57 G57 G57 12 Workpiece coordinate system selection 4
G58 G58 G58 12 Workpiece coordinate system selection 5
G59 G59 G59 12 Workpiece coordinate system selection 6
G61 G61 G61 13 Exact stop check mode 7.9
G64 G64 G64 13 Cutting mode 7.10
G65 G65 G65 00 Macro call 13.7.1
G66 G66 G66 14 Macro modal call A
G66.1 G66.1 G66.1 14 Macro modal call B
G67 G67 G67 14 Macro modal call cancel
G68 G68 G68 15 Facing turret mirror image ON 13.8
G69 G69 G69 15 Facing turret mirror image OFF
G70 G70 G72 09 Finishing cycle 13.2.4
G71 G71 G73 09 Longitudinal rough cutting cycle 13.2.1
G72 G72 G74 09 Face rough cutting cycle 13.2.2
G73 G73 G75 09 Stock removal in rough cutting cycle 13.2.3
3.6 G Code System
Reference
section in this
manual
(Section)
Automatic tool length offset, automatic tool
length measurement
Tool nose R compensation
(automatic selection of direction) ON
Coordinate system setting
Spindle clamp speed setting
16.3
12.4
14.6
10.4
11
3. DATA FORMATS
G code system (standard = 2) Group Function name
G74 G74 G76 09 Face cut-off cycle 13.2.5
G75 G75 G77 09 Longitudinal cut-off cycle 13.2.6
G76 G76 G78 09 Compound thread cutting cycle 13.2.7
G76.1 G76.1 G76.1 09 2-system simultaneous thread cutting cycle 1 17.13
G76.2 G76.2 G76.2 09 2-system simultaneous thread cutting cycle 2
G80 G80 G80 09 Hole drilling cycle cancel 13.3.4
G83 G83 G83 09 Deep hole drilling cycle 1 (Z axis) 13.3.1
G79 G83.2 G83.2 09 Deep hole drilling cycle 2 13.4
G84 G84 G84 09 Tap cycle (Z axis) 13.3.2
G85 G85 G85 09 Boring cycle (Z axis) 13.3.3
G87 G87 G87 09 Deep hole drilling cycle (X axis) 13.3.1
G88 G88 G88 09 Tap cycle (X axis) 13.3.2
G89 G89 G89 09 Boring cycle (X axis) 13.3.3
G90 G77 G20 09 Longitudinal cutting fixed cycle 13.1.1
G92 G78 G21 09 Thread cutting fixed cycle 13.1.2
G94 G79 G24 09 Face cutting fixed cycle 13.1.3
G96 G96 G96 17 Constant surface speed control 10.3
G97 G97 G97 17 Constant surface speed control cancel
G98 G94 G94 05 Asynchronous feed 7.3
G99 G95 G95 05 Synchronous feed
G110 G110 G110 00 Cross machining command 17.6
G111 G111 G111 00 Axis name change 18.3
G113 G113 G113 00
G114.1 G114.1 G114.1 00 Spindle synchronization 17.8
G114.2 G114.2 G114.2 00
G114.3 G114.3 G114.3 00
G115 G115 G115 00 Waiting at designated start point 1 17.2
G116 G116 G116 00 Waiting at designated start point 2 17.3
G117 G117 G117 00
G125 G125 G125 00 Control axis synchronization 17.7
G126 G126 G126 00 Control axis superimposition 17.11
G164 G164 G164 00 Spindle superimposition 17.12
G173 G173 G173 00 Inclined coordinate rotation control 13.16
G200 to G200 to G999 G macro call 18.3
3.6 G Code System
Reference
section in this
manual
(Section)
– G90 G90 03 Absolute value command
– G91 G91 03 Incremental value command
– G98 G98 10 Hole drilling cycle initial return 13.3
– G99 G99 10 Hole drilling cycle reference point return
Spindle synchronization, tool/spindle
synchronization cancel
Tool/spindle synchronization 1 (polygon
machining)
Tool/spindle synchronization 2 (hobb
machining)
Miscellaneous function output during axis
movement
5.1
17.8-17.12
17.9
17.10
18.1, 18.2
12
3. DATA FORMATS
(Note 1) The " " mark denotes a G code which is selected within each group when the power
3.6 G Code System
is turned ON or when resetting that initializes the modal commands is executed.
(Note 2) The "
" mark denotes a G code for which a parameter can be selected as the initial
status when the power is turned ON or when resetting that initializes the modal
commands is executed. Note that the inch/metric conversion can be made only when
the power is turned ON.
CAUTION
The commands with "no value after G", will be handled as "G00" during operation.
13
3. DATA FORMATS
3.7 Precautions Before Machining
Precautions before machining
CAUTION
Before starting actual machining, always carry out dry operation to confirm the machining
program, tool offset amount and workpiece offset amount, etc.
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.
3.7 Precautions Before Machining
14
Loading...