mitsubishi 700, 70 Programming Manual
MELDAS is a registered trademark of Mitsubishi Electric Corporation.
Other company and product names that appear in this manual are trademarks or registered
trademarks of the respective companies.
Introduction
This manual is a guide for using the MITSUBISHI CNC 700/70 Series.
Programming is described in this manual, so read this manual thoroughly before starting
programming. Thoroughly study the "Precautions for Safety" on the following page to
ensure safe use of this NC unit.
Details described in this manual
CAUTION
For items described in "Restrictions" or "Usable State", the instruction manual issued by the machine
tool builder takes precedence over this manual.
An effort has been made to note as many special handling methods in this user's manual. Items not
described in this manual must be interpreted as "not possible".
This manual has been writt e n o n t h e a ss u m p t i o n t h a t a l l o p t i on f u n c t i on s a r e added. Refer to the
specifications issued by the machine tool builder before starting use.
Refer to the Instruction Manual issued by each machine tool builder for details on each machine tool.
Some screens and functions may differ depending on the NC system or its version, and some
functions may not be possible. Please confirm the specifications before use.
General precautions
(1) Refer to the following documents for details on handling
MITSUBISHI CNC 700/70 Series Instruction Manual ................................. IB-1500042
Precautions for Safety
Always read the specifications issued by the machine maker, this manual, related manuals
and attached documents before installation, operation, programming, maintenance or
inspection to ensure correct use.
Understand this numerical controller, safety items and cautions before using the unit.
This manual ranks the safety precautions into "DANGER", "WARNING" and "CAUTION".
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.
Not applicable in this manual.
Not applicable in this manual.
1. Items related to product and manual
For items described as "Restrictions" or "Usable State" in this manual, the instruction manual
issued by the machine tool builder takes precedence over this manual.
An effort has been made to describe special handling of this machine, but items that are not
described must be interpreted as "not possible".
This manual is written on the assumption that all option functions are added. Refer to the
specifications issued by the machine tool builder before starting use.
Refer to the Instruction Manual issued by each machine tool builder for details on each
machine tool.
Some screens and functions may differ depending on the NC system or its version, and some
functions may not be possible. Please confirm the specifications before use.
DANGER
WARNING
CAUTION
(Continued on next page)
2. Items related to operation
Before starting actual machining, always carry out dry operation to confirm the machining
program, tool compensation amount and workpiece offset amount, etc.
If the workpiece coordinate system offset amount is changed during single block stop, the new
setting will be valid from the next block.
Turn the mirror image ON and OFF at the mirror image center.
Refer to the Instruction Manual issued by each machine tool builder for details on each
machine tool.
If the tool compensation amount is changed during automatic operation (including during single
block stop), it will be validated from the next block or blocks onwards.
3. Items related to programming
CAUTION
The commands with "no value after G" will be handled as "G00".
“EOB", "%", and “EOR” are symbols used for explanation. The actual codes for ISO are "CR,
LF" ("LF") and "%".
The programs created on the Edit screen are stored in the NC memory in a "CR, LF" format,
however, the programs created with external devices such as the FLD or RS-232C may be
stored in an "LF" format.
The actual codes for EIA are "EOB (End of Block)" and "EOR (End of Record)".
When creating the machining program, select the appropriate machining conditions, and make
sure that the performance, capacity and limits of the machine and NC are not exceeded. The
examples do not consider the machining conditions.
Do not change fixed cycle programs without the prior approval of the machine tool builder.
When programming a program of the multi-part system, carefully observe the movements
caused by other part systems' programs.
Contents
1. Control Axes..................................................................................................................................1
1.1 Coordinate Words and Control Axis........................................................................................1
1.2 Coordinate Systems and Coordinate Zero Point Symbols......................................................2
2. Least Command Increments........................................................................................................3
2.1 Input Setting Units...................................................................................................................3
2.2 Input Command Increment Tenfold.........................................................................................5
2.3 Indexing Increment..................................................................................................................6
3. Data Formats.................................................................................................................................7
3.1 Tape Codes.............................................................................................................................7
3.2 Program Formats ..................................................................................................................10
3.3 Tape Memory Format............................................................................................................13
3.4 Optional Block Skip...............................................................................................................13
3.4.1 Optional Block Skip; /......................................................................................................13
3.4.2 Optional Block Skip Addition ; /n.....................................................................................14
3.5 Program/Sequence/Block Numbers ; O, N ...........................................................................16
3.6 Parity H/V..............................................................................................................................17
3.7 G Code Lists .........................................................................................................................18
3.8 Precautions Before Starting Machining.................................................................................21
4. Buffer Register............................................................................................................................22
4.1 Input Buffer............................................................................................................................22
4.2 Pre-read Buffers....................................................................................................................23
5. Position Commands ...................................................................................................................24
5.1 Position Command Methods ; G90, G91 ..............................................................................24
5.2 Inch/Metric Command Change; G20, G21............................................................................26
5.3 Decimal Point Input...............................................................................................................28
6. Interpolation Functions..............................................................................................................33
6.1 Positioning (Rapid Traverse); G00........................................................................................33
6.2 Linear Interpolation; G01.......................................................................................................40
6.3 Plane Selection; G17, G18, G19...........................................................................................42
6.4 Circular Interpolation; G02, G03...........................................................................................44
6.5 R-specified Circular Interpolation; G02, G03........................................................................49
6.6 Helical Interpolation ; G17 to G19, G02, G03 .......................................................................52
6.7 Thread Cutting ......................................................................................................................56
6.7.1 Constant Lead Thread Cutting ; G33..............................................................................56
6.7.2 Inch Thread Cutting; G33................................................................................................60
6.8 Unidirectional Positioning; G60.............................................................................................61
6.9 Cylindrical Interpolation; G07.1.............................................................................................63
6.10 Polar Coordinate Interpolation; G12.1, G13.1/G112,G113.................................................71
6.11 Exponential Function Interpolation; G02.3, G03.3..............................................................78
6.12 Polar Coordinate Command ; G16/G15..............................................................................84
6.13 Spiral/Conical Interpolation; G02.0/G03.1(Type1), G02/G03(Type2).................................90
6.14 3-dimensional Circular Interpolation; G02.4, G03.4............................................................95
6.15 NURBS Interpolation.........................................................................................................100
6.16 Hypothetical Axis Interpolation; G07.................................................................................105
7. Feed Functions .........................................................................................................................107
7.1 Rapid Traverse Rate...........................................................................................................107
7.2 Cutting Feedrate .................................................................................................................107
7.3 F1-digit Feed.......................................................................................................................108
7.4 Feed Per Minute/Feed Per Revolution
(Asynchronous Feed/Synchronous Feed); G94, G95.........................................................110
7.5 Inverse Time Feed; G93 .....................................................................................................112
7.6 Feedrate Designation and Effects on Control Axes............................................................116
7.7 Rapid Traverse Constant Inclination Acceleration/Deceleration.........................................120
7.8 Rapid Traverse Constant Inclination Multi-step Acceleration/Deceleration........................122
7.9 Exact Stop Check; G09.......................................................................................................131
7.10 Exact Stop Check Mode; G61...........................................................................................134
7.11 Deceleration Check...........................................................................................................134
7.11.1 G1 -> G0 Deceleration Check.....................................................................................136
7.11.2 G1 -> G1 Deceleration Check.....................................................................................137
7.12 Automatic Corner Override; G62.......................................................................................138
7.13 Tapping Mode; G63 ..........................................................................................................143
7.14 Cutting Mode ; G64...........................................................................................................143
8. Dwell...........................................................................................................................................144
8.1 Per-second Dwell ; G04......................................................................................................144
9. Miscellaneous Functions .........................................................................................................146
9.1 Miscellaneous Functions (M8-digits BCD)..........................................................................146
9.2 Secondary Miscellaneous Functions (B8-digits, A8 or C8-digits).......................................148
9.3 Index Table Indexing...........................................................................................................149
10. Spindle Functions...................................................................................................................151
10.1 Spindle Functions (S6-digits Analog)................................................................................151
10.2 Spindle Functions (S8-digits) ............................................................................................151
10.3 Constant Surface Speed Control; G96, G97.....................................................................152
10.3.1 Constant Surface Speed Control................................................................................152
10.4 Spindle Clamp Speed Setting; G92 ..................................................................................153
10.5 Spindle/C Axis Control ......................................................................................................154
10.6 Multiple Spindle Control ....................................................................................................157
10.6.1 Multiple Spindle Control II...........................................................................................158
11. Tool Functions (T command).................................................................................................160
11.1 Tool Functions (T8-digit BCD)...........................................................................................160
12. Tool Compensation Functions ..............................................................................................161
12.1 Tool Compensation...........................................................................................................161
12.2 Tool Length Compensation/Cancel; G43, G44/G49 .........................................................165
12.3 Tool Length Compensation in the Tool Axis Direction ; G43.1/G49..................................168
12.4 Tool Radius Compensation; G38, G39/G40/G41,G42......................................................175
12.4.1 Tool radius Compensation Operation.........................................................................176
12.4.2 Other Commands and Operations during Tool Radius Compensation.......................185
12.4.3 G41/G42 Commands and I, J, K Designation.............................................................194
12.4.4 Interrupts during Tool Radius Compensation.............................................................200
12.4.5 General Precautions for Tool Radius Compensation..................................................202
12.4.6 Changing of Compensation No. during Compensation Mode.....................................203
12.4.7 Start of Tool Radius Compensation and Z Axis Cut in Operation...............................205
12.4.8 Interference Check .....................................................................................................207
12.4.9 Diameter Designation of Compensation Amount........................................................214
12.4.10 Workpiece Coordinate Changing during Radius Compensation...............................216
12.5 Three-dimensional Tool Radius Compensation ; G40/G41,G42.......................................218
12.6 Tool Position Offset; G45 to G48......................................................................................229
12.7 Programmed Compensation Input ; G10, G11..................................................................236
12.8 Inputting the Tool Life Management Data; G10, G11 .......................................................241
12.8.1 Inputting the Tool Life Management Data by G10 L3 Command................................241
12.8.2 Inputting the Tool Life Management Data by G10 L30 Command..............................243
12.8.3 Precautions for Inputting the Tool Life Management Data..........................................246
13. Program Support Functions ..................................................................................................247
13.1 Fixed Cycles......................................................................................................................247
13.1.1 Standard Fixed Cycles; G80 to G89, G73, G74, G75, G76........................................247
13.1.2 Drilling Cycle with High-Speed Retract.......................................................................274
13.1.3 Initial Point and R Point Level Return; G98, G99........................................................277
13.1.4 Setting of Workpiece Coordinates in Fixed Cycle Mode.............................................278
13.2 Special Fixed Cycle; G34, G35, G36, G37.1 ....................................................................279
13.3 Subprogram Control; M98, M99, M198.............................................................................284
13.3.1 Calling Subprogram with M98 and M99 Commands ..................................................284
13.3.2 Calling Subprogram with M198 Commands ...............................................................289
13.3.3 Figure Rotation; M98 I_ J_ K_....................................................................................289
13.4 Variable Commands..........................................................................................................292
13.5 User Macro Specifications ................................................................................................297
13.5.1 User Macro Commands; G65, G66, G66.1, G67........................................................297
13.5.2 Macro Call Command .................................................................................................298
13.5.3 ASCII Code Macro......................................................................................................307
13.5.4 Variables.....................................................................................................................311
13.5.5 Types of Variables ......................................................................................................313
13.5.6 Arithmetic Commands.................................................................................................351
13.5.7 Control Commands.....................................................................................................356
13.5.8 External Output Commands........................................................................................359
13.5.9 Precautions.................................................................................................................361
13.5.10 Actual Examples of Using User Macros....................................................................363
13.6 G Command Mirror Image; G50.1, G51.1.........................................................................367
13.7 Corner Chamfering/Corner Rounding I.............................................................................370
13.7.1 Corner Chamfering " ,C_ "..........................................................................................370
13.7.2 Corner Rounding " ,R_ ".............................................................................................372
13.8 Linear Angle Command ....................................................................................................373
13.9 Geometric Command........................................................................................................374
13.10 Circle Cutting; G12, G13.................................................................................................378
13.11 Parameter Input by Program; G10, G11.........................................................................380
13.12 Macro Interrupt; M96, M97..............................................................................................381
13.13 Tool Change Position Return; G30.1 to G30.6 ...............................................................389
13.14 Normal Line Control ; G40.1/G41.1/G42.1......................................................................392
13.15 High-accuracy Control ; G61.1, G08...............................................................................403
13.16 High-speed Machining Mode ; G05, G05.1.....................................................................417
13.16.1 High-speed Machining Mode I,II ; G05 P1, G05 P2..................................................417
13.17 High-speed High-accuracy Control ; G05, G05.1............................................................420
13.17.1 High-speed High-accuracy Control I, II.....................................................................420
13.17.2 SSS Control ..............................................................................................................427
13.18 Spline; G05.1 ..................................................................................................................432
13.19 High-accuracy Spline Interpolation ; G61.2.....................................................................439
13.20 Scaling ; G50/G51...........................................................................................................441
13.21 Coordinate Rotation by Program; G68/G69....................................................................446
13.22 Coordinate Rotation Input by Parameter; G10................................................................453
13.23 3-dimensional Coordinate Conversion ; G68/69.............................................................456
13.24 Tool Center Point Control; G43.4/G43.5.........................................................................473
13.25 Timing-synchronization between Part Systems..............................................................495
14. Coordinates System Setting Functions................................................................................498
14.1 Coordinate Words and Control Axes.................................................................................498
14.2 Basic Machine, Workpiece and Local Coordinate Systems..............................................499
14.3 Machine Zero Point and 2nd, 3rd, 4th Reference Positions..............................................500
14.4 Basic Machine Coordinate System Selection; G53...........................................................501
14.5 Coordinate System Setting ;G92.......................................................................................502
14.6 Automatic Coordinate System Setting ..............................................................................503
14.7 Reference (Zero) Position Return; G28, G29....................................................................504
14.8 2nd, 3rd and 4th Reference (Zero) Position Return; G30.................................................508
14.9 Reference Position Check; G27........................................................................................511
14.10 Workpiece Coordinate System Setting and Offset ; G54 to G59 (G54.1).......................512
14.11 Local Coordinate System Setting; G52...........................................................................524
14.12 Workpiece Coordinate System Preset; G92.1 ................................................................528
14.13 Coordinate System for Rotary Axis.................................................................................533
15. Measurement Support Functions..........................................................................................536
15.1 Automatic Tool Length Measurement; G37 ......................................................................536
15.2 Skip Function; G31............................................................................................................540
15.3 Multi-step Skip Function; G31.n, G04...............................................................................545
15.4 Multi-step Skip Function 2; G31........................................................................................547
15.5 Speed Change Skip; G31.................................................................................................549
15.6 Programmable Current Limitation .....................................................................................552
15.7 Stroke Check before Travel; G22/G23..............................................................................553
Appendix 1. Program Error .......................................................................................................555
Appendix 2. Order of G Function Command Priority..............................................................575
INDEX.............................................................................................................................................X-1
1. Control Axes
f
f
P
f
Di
1. Control Axes
1.1 Coordinate Words and Control Axis
Function and purpose
In the standard specifications, there are 3 control axes, but, by adding an additional axis, up to 4
axes can be controlled.
The designation of the processing direction responds to those axes and uses a coordinate word
made up of alphabet characters that have been decided beforehand.
X-Y table
+Z
+Y
+X
Program coordinates
Workpiece
1.1 Coordinate Words And Control Axis
+Z
X-Y table
+Y
Direction o
table movement
Bed
+X
Direction o
table movement
X-Y and revolving table
+Z
+Y
+C
+X
rogram coordinates
+X
Direction o
movement
table
+Y
Workpiece
+C
rection of table
revolution
1
1. Control Axes
Machi
1
1.2 Coordinate Systems And Coordinate Zero Point Symbols
1.2 Coordinate Systems and Coordinate Zero Point Symbols
Function and purpose
Workpiece
coordinate
system 3 (G56)
-X
: Reference position
: Machine coordinate zero point
: Workpiece coordinate zero points (G54 - G59)
Basic machine coordinate system
y
3
Workpiece
coordinate
system 2 (G55)
y
2
Workpiece
coordinate
system 1 (G54)
zero point
x1
y
1
st reference
position
ne
x
2
Local
coordinate
x
5
system
(G52)
y
-Y
x
Workpiece
coordinate
system 6 (G59)
x
3
Workpiece
coordinate
system 5 (G58)
y
5
Workpiece
coordinate
system 4
(G57)
2
2. Least Command Increments
2. Least Command Increments
2.1 Input Setting Units
Function and purpose
The input setting units are, as with the compensation amounts, the units of setting data used in
common for all axes.
The command units are the movement amounts in the program which are commanded with MDI
inputs or command tape. These are expressed with mm, inch or degree (°) units.
With the parameters, the command units are decided for each axis, and the input setting units are
decided commonly for all axes.
#1003 iunit = B
Input setting unit
Command unit
(Note 1) Inch/metric changeover is performed in either of 2 ways: conversion from the parameter
screen (#1041 I_inch: valid only when the power is turned ON) and conversion using the
G command (G20 or G21).
However, when a G command is used for the conversion, the conversion applies only to
the input command increments and not to the input setting units.
Consequently, the tool offset amounts and other compensation amounts as well as the
variable data should be preset to correspond to inches or millimeters.
(Note 2) The millimeter and inch systems cannot be used together.
(Note 3) During circular interpolation on an axis where the input command increments are
different, the center command (I, J, K) and the radius command (R) can be designated by
the input setting units. (Use a decimal point to avoid confusion.)
= C
= D
= E
#1015 cunit = 0 Follow #1003 iunit
= 1
= 10
= 100
= 1000
= 10000
Parameters
2.1 Input Setting Units
Linear axis
Millimeter Inch
0.001 0.0001 0.001
0.0001 0.00001 0.0001
0.00001 0.000001 0.00001
0.000001 0.0000001 0.000001
0.0001 0.00001 0.0001
0.001 0.0001 0.001
0.01 0.001 0.01
0.1 0.01 0.1
1.0 0.1 1.0
Rotation axis
(°)
3
2. Least Command Increments
Detailed description
(1) Units of various data
These input setting units determine the parameter setting unit, program command unit and the
external interface unit for the PLC axis and handle pulse, etc. The following rules show how the
unit of each data changes when the input setting unit is changed. This table applies to the NC
axis and PLC axis.
2.1 Input Setting Units
Data
Speed data
Example:
rapid
Position data
Example:
SoftLimit+
Interpolation
unit data
Unit
system
metre
Inch
metre
Inch
metre
Inch
(2) Program command
The program command unit follows the above table.
If the data has a decimal point, the number of digits in the integer section will remain and the
number of digits in the decimal point section will increase as the input setting unit becomes
smaller.
When setting data with no decimal point, and which is a position command, the data will be
affected by the input setting increment and input command increment.
For the feed rate, as the input setting unit becomes smaller, the number of digits in the integer
section will remain the same, but the number of digits in the decimal point section will increase.
Setting value
1µm (B) 0.1µm (C) 10nm (D) 1nm (E)
20000 (mm/min) 20000 20000 20000 20000Milli-
Setting range 1 to 999999 1 to 999999 1 to 999999 1 to 999999
2000 (inch/min) 2000 2000 2000 2000
Setting range 1 to 999999 1 to 999999 1 to 999999 1 to 999999
123.123 (mm) 123.123 123.1230 123.12300 123.123000MilliSetting range ±99999.999 ±99999.9999 ±99999.99999 ±99999.999999
12.1234 (inch) 12.1234 12.12340 12.123400 12.1234000
Setting range ±9999.9999 ±9999.99999 ±9999.999999 ±9999.9999999
1 (µm) 2 20 200 2000Milli-
Setting range ±9999 ±9999 ±9999 ±9999
0.001 (inch) 2 20 200 2000
Setting range ±9999 ±9999 ±9999 ±9999
Input setting unit
4
2. Least Command Increments
2.2 Input Command Increment Tenfold
Function and purpose
The program's command increment can be multiplied by an arbitrary scale with the parameter
designation.
This function is valid when a decimal point is not used for the command increment.
The scale is set with the parameters.
Detailed description
(1) When running a machining program already created with a 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", machining similar to before this function is possible.
(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", machining similar to before this function is possible.
(3) This function cannot be used for the dwell function G04_X_(P_);.
(4) This function cannot be used for the compensation amount of the tool compensation input.
(5) This function can be used when decimal point type I is valid, but cannot be used when decimal
point type II is valid.
Program example
(Machining program:
programmed with 1=10µm)
(CNC unit is 1=1µm system)
X Y X Y
N1 G90 G00 X0 Y0; 0 0 0 0
N2 G91 X-10000 Y-15000; -100.000 -150.000 -10.000 -15.000
N3 G01 X-10000 Y-5000 F500; -200.000 -200.000 -20.000 -20.000
N4 G03 X-10000 Y-10000 J-10000; -300.000 -300.000 -30.000 -30.000
N5 X10000 Y-10000 R5000; -200.000 -400.000 -20.000 -40.000
N6 G01 X20.000 Y.20.000 -180.000 -380.000 0.000 -20.000
-100 -200 -300
2.2 Input Command Increment Tenfold
"UNIT*10" parameter
10 1
-10 -20 -30
N6
N2
W
-10
-20
-30
-40
N4
R
N3
N5
N6
UNIT*10 ON
N1
N2
W
-100
-200
-300
-400
N1
N3
N4
N5
R
UNIT*10 OFF
5
2. Least Command Increments
2.3 Indexing Increment
Function and purpose
This function limits the command value for the rotary axis.
This can be used for indexing the rotary table, etc. It is possible to cause a program error with a
program command other than an indexing increment (parameter setting value).
Detailed description
When the indexing increment (parameter) for limiting the command value is set, the rotary axis can
be positioned with that indexing increment. If a program other than the indexing increment setting
value is commanded, a program error (P20) will occur.
The indexing position will not be checked when the parameter is set to 0.
(Example) When the indexing increment setting value is 2 degrees, only command with the
2-degree increment are possible.
G90 G01 C102. 000 ; … Moves to the 102 degree angle.
G90 G01 C101. 000 : … Program error
G90 G01 C102 ; … Moves to the 102 degree angle. (Decimal point type II)
The following axis specification parameter is used.
# Item Contents
2106 Index unit Indexing
Precautions
• When the indexing increment is set, degree increment positioning takes place.
• The indexing position is checked with the rotary axis, and is not checked with other axes.
• When the indexing increment is set to 2 degrees, the rotary axis is set to the B axis, and the B
axis is moved with JOG to the 1.234 position, an indexing error will occur if "G90B5." or "G91B5."
is commanded.
increment
2.3 Indexing Increment
Set the indexing increment to which the rotary
axis can be positioned.
Setting range
(unit)
0 to 360 (° )
6
3. Data Formats
3. Data Formats
3.1 Tape Codes
Function and purpose
The tape command codes used for this controller are combinations of alphabet letters (A, B, C, ...
Z), numbers (0, 1, 2 ... 9) and signs (+, -, / ...). These alphabet letters, numbers and signs are
referred to as characters. Each character is represented by a combination of 8 holes which may, or
may not, be present.
These combinations make up what is called codes.
This controller uses, the ISO code (R-840).
(Note 1) If a code not given in the tape code table in Fig. 1 is assigned during operation, program
(Note 2) For the sake of convenience, a semicolon " ; " has been used in the CNC display to
3.1 Tape Codes
error (P32) will result.
indicate the end of a block (EOB/IF) which separates one block from another. Do not use
the semicolon key, however, in actual programming but use the keys in the following
table instead.
CAUTION
“EOB", "%", and “EOR” are symbols used for explanation. The actual codes for ISO are
"CR, LF" ("LF") and "%".
The programs created on the Edit screen are stored in the NC memory in a "CR, LF" format,
however, the programs created with external devices such as the FLD or RS-232C may be
stored in an "LF" format.
The actual codes for EIA are "EOB (End of Block)" and "EOR (End of Record)".
Detailed description
EOB/EOR keys and displays
Code used
Key used
End of block LF or NL ;
End of record % %
(1) Significant data section (label skip function)
All data up to the first EOB ( ; ), after the power has been turned on or after operation has been
reset, are ignored during automatic operation based on tape, memory loading operation or
during a search operation. In other words, the significant data section of a tape extends from
the character or number code after the initial EOB ( ; ) code after resetting to the point where
the reset command is issued.
ISO Screen display
7
3. Data Formats
G
R
•••••••
•
•••
•
•
•••••••••
•
•••••••
•
•
•••••••••••••••••
•
•
•
•••••••••••••••
•••••••••
•
(2) Control out, control in
When the ISO code is used, all data between control out "(" and control in ")" or ";" are ignored,
although these data appear on the setting and display unit. Consequently, the command tape
name, No. and other such data not directly related to control can be inserted in this section.
This information (except (B) in the tape codes) will also be loaded, however, during tape
loading. The system is set to the "control in" mode when the power is witched on.
Example of ISO code
•
3.1 Tape Codes
•
•• ••
• • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • •
•••
•••
• •
• • •• •
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
••
•••••
•
•
(3) EOR (%) code
Generally, the end-or-record code is punched at both ends of the tape. It has the following
functions:
(a) Rewind stop when rewinding tape (with tape handler)
(b) Rewind start during tape search (with tape handler)
(c) Completion of loading during tape loading into memory
(4) Tape preparation for tape operation (with tape handler)
10cm
%
(EOR)
2m
If a tape handler is not used, there is no need for the 2-meter dummy at both ends of the tape
and for the head EOR (%) code.
• • • • • • • •
;;;;
Initial block
• • • • • • • • • • • • • • • •
(EOB)
Last block
(EOB)(EOB)
10cm %
(EOR)(EOB)
2m
8
3. Data Formats
A
Y
( (
)
) (
)
)
)
)
@
)
)
A
ISO code (R-840)
Feed holes
8 7 6 5 4 3 2 1
Channel No.
3.1 Tape Codes
•
•
•
•
•
•
•
••
•
••
••
•
• •
•• •
•• •• •
• •• ••
•• •• •
• •• • •
• •• ••
•• •• •••
• •
•• •
•• •
• •
•• •• •
• •• • •
• •• ••
•• •• •••
•• ••
• ••
• ••• •
•
•
•
•
•
•
•
•• ••• ••
•• ••• • •
•
• •• • •
• •
•
•
•
••
••
••
Code A are stored on tape but an error results (except when they are used in the comment
section) during operation.
The B codes are non-working codes and are always ignored. Parity V check is not executed.
•
•
•
•
•
•
•• •
•• • •
•• ••
•• •••
•
••
•
••
•
•
•
•
•
•
•
•
• •
•
••
•
•••
•
•
•
•
•
•
•
•
•• ••
•• • •
•• ••
•• •
•• •••
•• • •
•• •
•
•
•
•
••• •
•
•• •
••• • •
•
•
•
•
•
••
•
•
•
•
•••
••• ••
••• •
••• ••
••• •••
•
•
••• •••
•
••• •••
•
•
1
•
2
•
3
••
4
5
6
7
8
9
•
0
•
B
•
C
••
D
E
F
G
H
I
•
J
K
L
M
N
O
P
Q
•
R
•
S
••
T
U
V
W
X
•
Z
+
.
,
/
%
LF(Line Feed) or NL
Control Out
Control In
•
:
#
••
*
=
[
]
SP(Space
CR(Carriage Return)
BS(Back Space
HT(Horizontal Tab
•
&
!
•
$
' (Apostrophe)
;
<
>
?
"
•
DEL(Delete
NULL
DEL(Delete
• Under the ISO code, IF or NL is EOB and % is EOR.
• Under the ISO code, CR is meaningless, and EOB will not occur.
Table of tape codes
B
9
3. Data Formats
Alp
)
3.2 Program Formats
Function and purpose
The prescribed arrangement used when assigning control information to the controller is known as
the program format, and the format used with this controller is called the "word address format".
Detailed descripti on
(1) Word and address
A word is a collection of characters arranged in a specific sequence. This entity is used as the
unit for processing data and for causing the machine to execute specific operations. Each
word used for this controller consists of an alphabet letter and a number of several digits
(sometimes with a "-" sign placed at the head of the number.).
3.2 Program Formats
Word
*
Numerals
habet (address
Word configuration
The alphabet letter at the head of the word is the address. It defines the meaning of the
numerical information which follows it.
For details of the types of words and the number of significant digits of words used for this
controller, refer to the "format details".
(2) Blocks
A block is a collection of words. It includes the information which is required for the machine to
execute specific operations. One block unit constitutes a complete command. The end of each
block is marked with an EOB (end-of-block) code.
(Example 1)
G0X - 1000 ;
G1X - 2000F500 ;
(Example 2)
(G0X - 1000 ; )
G1X - 2000F500 ;
(3) Programs
A program is a collection of several blocks.
2 blocks
Since the semicolon in the parentheses will not result
in an EOB, it is 1 block.
10
3. Data Formats
<Brief summary of format details>
Program No. 08
Sequence No. N6
Preparatory function G3/G21
Movement
axis
Arc and
cutter
radius
Dwell
Feed
function
(Feed per
minute)
Feed
function
(Feed per
revolution)
Tool compensation
Miscellaneous function (M)
Spindle function (S)
Tool function (T)
2nd miscellaneous function A8/B8/C8
Subprogram
Fixed
cycle
0.001(°) mm/
0.001 inch
0.0001(°) mm/
0.0001 inch
0.00001(°) mm/
0.00001 inch
0.000001(°) mm/
0.000001 inch
0.001(°) mm/
0.001 inch
0.0001(°) mm/
0.0001 inch
0.00001(°) mm/
0.00001 inch
0.000001(°) mm/
0.000001 inch
0.001(rev)/(s)
0.001(°) mm/
0.001 inch
0.0001 (°) mm/
0.0001 inch
0.00001 (°) mm/
0.00001 inch
0.000001 (°) mm/
0.000001 inch
0.0001(°) mm/
0.0001 inch
0.00001 (°) mm/
0.00001 inch
0.000001 (°) mm/
0.000001 inch
0.0000001 (°) mm/
0.0000001 inch
0.001(°) mm/
0.001 inch
0.0001(°) mm/
0.0001 inch
0.00001(°) mm/
0.00001 inch
0.000001(°) mm/
0.000001 inch
Metric command Inch command
X+53 Y+53 Z+53 α+53 X+44 Y+44 Z+44 α+44 X+53 Y+53 Z+53 α+53 X+53 Y+53 Z+53 α+53
X+54 Y+54 Z+54 α+54 X+45 Y+45 Z+45 α+45 X+54 Y+54 Z+54 α+54 X+54 Y+54 Z+54 α+54
X+55 Y+55 Z+55 α+55 X+46 Y+46 Z+46 α+46 X+55 Y+55 Z+55 α+55 X+55 Y+55 Z+55 α+55
X+56 Y+56 Z+56 α+56 X+47 Y+47 Z+47 α+47 X+56 Y+56 Z+56 α+56 X+56 Y+56 Z+56 α+56
I+53 J+53 K+53 I+44 J+44 K+44 I+53 J+53 K+53
I+54 J+54 K+54 I+45 J+45 K+45 I+54 J+54 K+54
I+55 J+55 K+55 I+46 J+46 K+46 I+55 J+55 K+55
I+56 J+56 K+56 I+47 J+47 K+47 I+56 J+56 K+56
X53/P8
F63 F54 F63 F54 (Note 6)
F64 F55 F64 F55 (Note 6)
F65 F56 F65 F56 (Note 6)
F66 F57 F66 F57 (Note 6)
F33 F34 F33 F34 (Note 6)
F34 F35 F34 F35 (Note 6)
F35 F36 F35 F36 (Note 6)
F36 F37 F36 F37 (Note 6)
H3 D3
M8
S8
T8
P8 H5 L4
R+53 Q53 P8 L4 R+44 Q44 P8 L4 R+53 Q53 P8 L4 R+53 Q53 P8 L4
R+54 Q54 P8 L4 R+45 Q45 P8 L4 R+54 Q54 P8 L4 R+54 Q54 P8 L4
R+55 Q55 P8 L4 R+46 Q46 P8 L4 R+55 Q55 P8 L4 R+55 Q55 P8 L4
R+56 Q56 P8 L4 R+47 Q47 P8 L4 R+56 Q56 P8 L4 R+56 Q56 P8 L4
3.2 Program Formats
Rotary axis
(Metric command)
← ← ←
← ← ←
← ← ←
← ← ←
← ← ←
← ← ←
← ← ←
← ← ←
← ← ←
← ← ←
Rotary axis
(Inch command)
I+53 J+53 K+53
I+54 J+54 K+54
I+55 J+55 K+55
I+56 J+56 K+56
(Note 5)
(Note 5)
(Note 5)
(Note 5)
(Note 1) α indicates the additional axis address, such as A, B or C.
(Note 2) The number of digits check for a word is carried out with the maximum number of digits of that address.
(Note 3) Numerals can be used without the leading zeros.
11
3. Data Formats
3.2 Program Formats
(Note 4) The description of the brief summary is explained below:
Example 1 : 08 :8-digit program No.
Example 2 : G21 :Dimension G is 2 digits to the left of the decimal point, and 1 digit to the right.
Example 3 : X+53 :Dimension X uses + or - sign and represents 5 digits to the left of the decimal
point and 3 digits to the right.
For example, the case for when the X axis is positioned (G00) to the 45.123 mm
position in the absolute value (G90) mode is as follows:
G00 X45.123 ;
3 digits below the decimal point
5 digits above the decimal point, so it's +00045, but the
leading zeros and the mark (+) have been omitted.
G0 is possible, too.
(Note 5) If an arc is commanded using a rotary axis and linear axis while inch commands are being used, the
degrees will be converted into 0.1 inches for interpolation.
(Note 6) While inch commands are being used, the rotary axis speed will be in increments of 10 degrees.
Example: With the F1. (per-minute-feed) command, this will become the 10 degrees/minute command.
(Note 7) The decimal places below the decimal point are ignored when a command, such as an S command,
with an invalid decimal point has been assigned with a decimal point.
(Note 8) This format is the same for the value input from the memory, MDI or setting and display unit.
(Note 9) Command the program No. in an independent block. Command the program No. in the head block of
the program.
12
3. Data Formats
3.3 Tape Memory Format
Function and purpose
(1) Storage tape and significant sections
The others are about from the current tape position to the EOB. Accordingly, under normal
conditions, operate the tape memory after resetting.
The significant codes listed in "Table of tape codes" in "3.1 Tape Codes" in the above
significant section are actually stored into the memory. All other codes are ignored and are not
stored.
The data between control out "(" and control in ")" are stored into the memory.
3.4 Optional Block Skip
3.4.1 Optional Block Skip; /
Function and purpose
This function selectively ignores specific blocks in a machining program which starts with the "/"
(slash) code.
Detailed description
3.3 Tape Memory Format
(1) Provided that the optional block skip switch is ON, blocks starting with the "/" code are ignored.
They are executed if the switch is OFF.
Parity check is valid regardless of whether the optional block skip switch is ON or OFF.
When, for instance, all blocks are to be executed for one workpiece but specific block are not
to be executed for another workpiece, the same command tape can be used to machine
different parts by inserting the "/" code at the head of those specific blocks.
Precautions for using optional block skip
(1) Put the "/" code for optional block skip at the beginning of a block. If it is placed inside the block,
it is assumed as a user macro, a division instruction.
Example : N20 G1 X25./Y25. ;....NG (User macro, a division instruction; a program error
results.)
/N20 G1 X25. Y25. ;.....OK
(2) Parity checks (H and V) are conducted regardless of the optional block skip switch position.
(3) The optional block skip is processed immediately before the pre-read buffer.
Consequently, it is not possible to skip up to the block which has been read into the pre-read
buffer.
(4) This function is valid even during a sequence number search.
(5) All blocks with the "/" code are also input and output during tape storing and tape output,
regardless of the position of the optional block skip switch.
13
3. Data Formats
3.4.2 Optional Block Skip Addition ; /n
Function and purpose
Whether the block with "/n (n:1 to 9)" (slash) is executed during automatic operation and searching
is selected.
By using the machining program with "/n" code, different parts can be machined by the same
program.
Detailed description
The block with "/n" (slash) code is skipped when the "/n" is programmed to the head of the block
and the optional block skip signal is turned ON.
For the block with the "/n" code inside the block (not the head of block), the program is operated
according to the value of the parameter "#1226 aux10/bit1" setting.
When the optional block skip signal is OFF, the block with "/n" is executed.
Example of program
(1) When the 2 parts like the figure below are machined, the following program is used. When the
optional block skip 5 signal is ON, the part 1 is created. When the optional block skip 5 signal is
OFF, the part 2 is created.
<Program>
N1 G54;
N2 G90G81X50. Z-20. R3. F100;
/5 N3 X30.;
N4 X10.;
N5 G80;
M02;
Part 1
the optional block skip 5 signal ON
3.4 Optional Block Skip
Part 2
the optional block skip 5 signal OFF
N4 N2 N2 N3
14
N4
3. Data Formats
3.4 Optional Block Skip
(2) When two or more "/n" codes are commanded to the head of the same block, the block is
ignored if either of the optional block skip signal corresponding to the command is ON.
<Program>
N01 G90 Z3. M03 S1000;
/1/2 N02 G00 X50.;
/1/2 N03 G01 Z-20. F100;
/1/2 N04 G00 Z3.;
/1 /3 N05 G00 X30.;
/1 /3 N06 G01 Z-20. F100;
/1 /3 N07 G00 Z3.;
/2/3 N08 G00 X10.;
/2/3 N09 G01 Z-20. F100;
/2/3 N10 G00 Z3.;
N11 G28 X0 M05;
(a) Optional block skip 1 signal ON
(Optional block skip 2, 3 signals OFF)
N01 -> N08 -> N09 -> N10 -> N11 -> N12
(b) Optional block skip 2 signal ON
(Optional block skip 1, 3 signals OFF)
N01 -> N05 -> N06 -> N07 -> N11 -> N12
(c) Optional block skip 3 signal ON
(Optional block skip 1, 2 signals OFF)
N01 -> N02 -> N03 -> N04 -> N11 -> N12
N12 M02;
(3) When the parameter "#1226 aux10/bit1" is "1", when two or more "/n" are commanded inside
the same block, the commands following "/n" in the block are ignored if either of the optional
block skip signal corresponding to the command is ON.
N01 G91 G28 X0.Y0.Z0.;
N02 G01 F1000;
N03 X1. /1 Y1. /2 Z1.;
N04 M30;
(a) When the optional block skip 1 signal is
ON and the optional block skip 2 signal is
OFF, "Y1. Z1." is ignored
(b) When the optional block skip 1 signal is
OFF and the optional block skip 2 signal is
ON, "Z1." is ignored.
15
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 "0" followed by a number with up to 8 digits.
(2) Sequence numbers are attached where appropriate to command blocks which configure
machining programs, and they are designated by the address "N" followed by a number with
up to 6 digits.
(3) Block numbers are automatically provided internally. They are preset to zero every time a
program number or sequence number is read, and they are counted up one at a time unless
program numbers or sequence numbers are commanded in blocks which are subsequently
read.
Consequently, all the blocks of the machining programs given in the table below can be
determined without further consideration by combinations of program numbers, sequence
numbers and block numbers.
Machining program
O12345678 (DEMO, PROG) ; 12345678 0 0
G92 X0 Y0 ; 12345678 0 1
G90 G51 X-150. P0.75 ; 12345678 0 2
N100 G00 X-50. Y-25. ; 12345678 100 0
N110 G01 X250. F300 ; 12345678 110 0
Y-225. ; 12345678 110 1
X-50. ; 12345678 110 2
Y-25.; 12345678 110 3
N120 G51 Y-125. P0.5 ; 12345678 120 0
N130 G00 X-100. Y-75. ; 12345678 130 0
N140 G01 X-200. ; 12345678 140 0
Y-175. ; 12345678 140 1
X-100. ; 12345678 140 2
Y-75. ; 12345678 140 3
N150 G00 G50 X0 Y0 ; 12345678 150 0
N160 M02 ; 12345678 160 0
%
Program No. Sequence No. Block No.
Monitor display
16
3. Data Formats
•
•
• • •
• • • • • • • • • • • • •
•
•
• •
•
•
• • •
• • •
• •
•
• • •
•
• •
•
• • • • • • • • •
•
• •
• • •
3.6 Parity H/V
Function and purpose
Parity check provides a mean of checking whether the tape has been correctly perforated or not.
This involves checking for perforated code errors or, in other words, for perforation errors. There
are two types of parity check: Parity H and Parity V.
(1) Parity H
3.6 Parity H/V
Parity H checks the number of holes configuring a character and it is done during tape
operation, tape input and sequence number search.
A parity H error is caused in the following cases.
(a) ISO code
When a code with an odd number of holes in a significant data section has been detected.
(b) EIA code
When a code with an even number of holes in a significant data section has been
detected.
Parity H error example
• • • •
•
• • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • • •
• • • • • • • • • • • • • • •
•
•
• • • • • • • • •
• • •
(2) Parity V
• • • • •
• • • • • • • • • • • • • • • • •
• • • • • • • • • • • • • •
When a parity H error occurs, the tape stops following the alarm code.
A parity V check is done during tape operation, tape input and sequence number search when
the I/O PARA #9n15 (n is the unit No.1 to 5) parity V check function is set to "1". It is not done
during memory operation.
A parity V error occurs in the following case: when the number of codes from the first
significant code to the EOB (;) in the significant data section in the vertical direction of the tape
is an odd number, that is, when the number of characters in one block is odd.
When a parity V error is detected, the tape stops at the code following the EOB (;).
(Note 1) Among the tape codes, there are codes which are counted as characters for parity
(Note 2) Any space codes which may appear within the section from the initial EOB code to
• •
• • • • • • • • • •
•
•
• • • •
• • •
• • • • • • •
This character causes a parity H error.
and codes which are not counted as such. For details, refer to the "Table of tape
codes" in "3.1 Tape Codes".
the address code or "/" code are counted for parity V check.
17
3. Data Formats
3.7 G Code Lists
Function and purpose
G code Group Function Section
Δ 00 01 Positioning 6.1
Δ 01 01 Linear interpolation 6.2
02 01 Circular interpolation CW (clockwise)
03 01 Circular interpolation CCW (counterclockwise)
02.1 01 Spiral/Conical interpolation CW (type1) 6.13
03.1 01 Spiral/Conical interpolation CCW (type1) 6.13
02.3 01 Exponential function interpolation positive rotation 6.11
03.3 01 Exponential function interpolation negative rotation 6.11
02.4 01 3-dimensional circular interpolation 6.14
03.4 01 3-dimensional circular interpolation 6.14
04 00 Dwell 8.1
05 00 High-speed machining mode
05.1 00 High-speed high-accuracy control I
06.2 01 NURBS interpolation 6.15
07 00
07.1
107
08 00 High-accuracy control 13.15
09 00 Exact stop check 7.9
10 00 Program data input (parameter /compensation data/parameter
11 00 Program data input cancel 12.7
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 6.3
Δ 18 02 Plane selection Z-X 6.3
Δ 19 02 Plane selection Y-Z 6.3
Δ 20 06 Inch command 5.2
Δ 21 06 Metric command 5.2
R-specified circular interpolation CW
Helical interpolation CW
Spiral/Conical interpolation CW (type 2)
R-specified circular interpolation CCW
Helical interpolation CCW
Spiral/Conical interpolation CCW (type 2)
High-speed high-accuracy control II
Spline
Hypothetical axis interpolation 6.16
21 Cylindrical interpolation
coordinate rotation data)
21 Polar coordinate interpolation ON
21 Polar coordinate interpolation cancel
3.7 G Code Lists
6.4
6.5
6.6
6.13
6.4
6.5
6.6
6.13
13.16
13.17
13.17
13.18
6.9
12.7
13.11
13.22
13.11
6.10
6.10
18
Loading...