MITSUBISHI CNC M700V, M70V 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 M700V/M70 Series.

Programming for M2/M0 format is described in this manual, so read this manual thoroughly before starting programming. Thoroughly study the "Precautions for Safety" on the following page to ensure safe use of this NC unit.

Details described in this manual

CAUTION

For items described in "Restrictions" or "Usable State", the instruction manual issued by the machine tool builder takes precedence over this manual.

An effort has been made to note as many special handling methods in this user's manual. Items not described in this manual must be interpreted as "not possible".

This manual has been written on the assumption that all option functions are added. Refer to the specifications issued by the machine tool builder before starting use.

Refer to the Instruction Manual issued by each machine tool builder for details on each machine tool.

Some screens and functions may differ depending on the NC system or its version, and some functions may not be possible. Please confirm the specifications before use.

General precautions
(1) Refer to the following documents for details on handling
MITSUBISHI CNC M700V/M70 Series Instruction Manual .........................	IB-1500922

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

When the user may be subject to imminent fatalities or major injuries if handling is mistaken.

When the user may be subject to fatalities or major injuries if handling is mistaken.

When the user may be subject to injuries or when physical damage may occur if handling is mistaken.

Note that even items ranked as " CAUTION", may lead to major results depending on the situation. In any case, important information that must always be observed is described.

DANGER

Not applicable in this manual.

WARNING

1. Items related to operation

If the operation start position is set in a block which is in the middle of the program and the program is started, the program before the set block is not executed. Please confirm that G and F modal and coordinate values are appropriate. If there are coordinate system shift commands or M, S, T and B commands before the block set as the start position, carry out the required commands using the MDI, etc. If the program is run from the set block without carrying out these operations, there is a danger of interference with the machine or of machine operation at an unexpected speed, which may result in breakage of tools or machine tool or may cause damage to the operators.

Under the constant surface speed control (during G96 modal), if the axis targeted for the constant surface speed control moves toward the spindle center, the spindle rotation speed will increase and may exceed the allowable speed of the workpiece or chuck, etc. In this case, the workpiece, etc. may jump out during machining, which may result in breakage of tools or machine tool or may cause damage to the operators.

CAUTION

1. Items related to product and manual

For items described as "Restrictions" or "Usable State" in this manual, the instruction manual issued by the machine tool builder takes precedence over this manual.

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.

2. Items related to operation

Before starting actual machining, always carry out dry operation to confirm the machining program, tool compensation amount and workpiece offset amount, etc.

If the workpiece coordinate system offset amount is changed during single block stop, the new setting will be valid from the next block.

Turn the mirror image ON and OFF at the mirror image center.

Refer to the Instruction Manual issued by each machine tool builder for details on each machine tool.

If the tool compensation amount is changed during automatic operation (including during single block stop), it will be validated from the next block or blocks onwards.

3. Items related to programming

The commands with "no value after G" will be handled as "G00".

“EOB", "%", and “EOR” are symbols used for explanation. The actual codes for ISO are "CR, LF" ("LF") and "%".

The programs created on the Edit screen are stored in the NC memory in a "CR, LF" format, however, the programs created with external devices such as the FLD or RS-232C may be stored in an "LF" format.

The actual codes for EIA are "EOB (End of Block)" and "EOR (End of Record)".

When creating the machining program, select the appropriate machining conditions, and make sure that the performance, capacity and limits of the machine and NC are not exceeded. The examples do not consider the machining conditions.

Do not change fixed cycle programs without the prior approval of the machine tool builder.

When programming a program of the multi-part system, carefully observe the movements caused by other part systems' programs.

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 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 ; L(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.....................................................................		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	Per-minute/Per-revolution Feed (Asynchronous/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 ...............................................................................................	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
10.4	Spindle Clamp Speed Setting; G92 ..................................................................................	154
10.5	Spindle/C Axis Control ......................................................................................................	156
10.6	Multiple Spindle Control ....................................................................................................	159
10.6.1 Multiple Spindle Control II...........................................................................................		160
11. Tool Functions (T command).................................................................................................		162
11.1	Tool Functions (T8-digit BCD)...........................................................................................	162
12. Tool Compensation Functions ..............................................................................................		163
12.1	Tool Compensation ...........................................................................................................	163
12.2	Tool Length Compensation/Cancel; G43/G44 ..................................................................	167
12.3	Tool Length Compensation in the Tool Axis Direction ; G43.1/G44..................................	170
12.4	Tool Radius Compensation; G38, G39/G40/G41,G42......................................................	177
12.4.1 Tool Radius Compensation Operation........................................................................		178
12.4.2 Other Commands and Operations During Tool Radius Compensation ......................		187
12.4.3 G41/G42 Commands and I, J, K Designation.............................................................		196
12.4.4 Interrupts During Tool Radius Compensation.............................................................		202
12.4.5 General Precautions for Tool Radius Compensation..................................................		204
12.4.6 Changing of Compensation No. During Compensation Mode ....................................		205
12.4.7 Start of Tool Radius Compensation and Z Axis Cut in Operation...............................		207
12.4.8 Interference Check .....................................................................................................		209
12.4.9 Diameter Designation of Compensation Amount........................................................		216
12.4.10 Workpiece Coordinate Changing During Radius Compensation..............................		218
12.5	Three-dimensional Tool Radius Compensation ; G40/G41,G42.......................................	220
12.6	Tool Position Offset; G45 to G48 ......................................................................................	231
12.7	Programmed Compensation Input; G10, G11.1................................................................	238
12.8	Compensation Data Input to Variable by Program; G11...................................................	243
12.9	Inputting the Tool Life Management Data; G10, G11 .......................................................	244
12.9.1 Inputting the Tool Life Management Data by G10 L3 Command................................		244
12.9.2 Inputting the Tool Life Management Data by G10 L30 Command..............................		246
12.9.3 Precautions for Inputting the Tool Life Management Data..........................................		249

13. Program Support Functions ..................................................................................................			250
13.1	Fixed Cycles......................................................................................................................		250
13.1.1 Standard Fixed Cycles; G80 to G89, G73, G74, G75, G76 ........................................			250
13.1.2 Drilling Cycle with High-Speed Retract.......................................................................			278
13.1.3 Initial Point and R Point Level Return; G98, G99........................................................			281
13.1.4 Setting of Workpiece Coordinates in Fixed Cycle Mode.............................................			283
13.2 Special Fixed Cycle; G34, G35, G36, G37 .......................................................................			284
13.3 Subprogram Control; G22, G22 ........................................................................................			289
13.3.1 Calling Subprogram with G22 and G22 Commands...................................................			289
13.3.2 Figure Rotation; G22 I_ J_ K_ ....................................................................................			293
13.4	Variable Commands..........................................................................................................		296
13.5	User Macro Specifications ................................................................................................		301
13.5.1 User Macro Commands; G65, G66, G66.1, G67, G68(G23)......................................			301
13.5.2		Macro Call Command .................................................................................................	302
13.5.3		ASCII Code Macro......................................................................................................	311
13.5.4		Variables.....................................................................................................................	315
13.5.5		Types of Variables ......................................................................................................	317
13.5.6		Arithmetic Commands.................................................................................................	355
13.5.7		Control Commands.....................................................................................................	360
13.5.8		External Output Commands........................................................................................	363
13.5.9		Precautions.................................................................................................................	365
13.5.10 Actual Examples of Using User Macros....................................................................			367
13.6 G Command Mirror Image; G50.1, G51.1 / G62 ...............................................................			371
13.7 Corner Chamfering/Corner Rounding I .............................................................................			374
13.7.1		Corner Chamfering " ,C_ " ..........................................................................................	374
13.7.2		Corner Rounding " ,R_ " .............................................................................................	376
13.8	Linear Angle Command ....................................................................................................		377
13.9	Geometric Command ........................................................................................................		378
13.10	Circle Cutting; G12, G13 .................................................................................................		382
13.11	Parameter Input by Program; G10, G11.1 ......................................................................		384
13.12	Macro Interrupt; ION, IOF ...............................................................................................		385
13.13	Tool Change Position Return; G30.1 to G30.6 ...............................................................		393
13.14	Normal Line Control ; G40.1/G41.1/G42.1......................................................................		396
13.15	High-accuracy Control ; G61.1, G08 ...............................................................................		407
13.16	High-speed Machining Mode; G05, G05.1......................................................................		421
13.16.1 High-speed Machining Mode I,II; G05 P1, G05 P2...................................................			421
13.17	High-speed High-accuracy Control; G05, G05.1.............................................................		424
13.17.1 High-speed High-accuracy Control I, II.....................................................................			424
13.17.2		SSS Control ..............................................................................................................	430
13.18	Spline; G05.1 ..................................................................................................................		435
13.19	High-accuracy Spline Interpolation ; G61.2.....................................................................		442
13.20	Scaling; G50/G51............................................................................................................		444
13.21	Coordinate Rotation by Program; G68.1/G69.1 ..............................................................		449
13.22	Coordinate Rotation Input by Parameter; G10................................................................		457
13.23	3-dimensional Coordinate Conversion; G68.1/69.1 ........................................................		460
13.24	Tool Center Point Control; G43.4/G43.5 .........................................................................		477
13.25	Timing-synchronization between Part Systems ..............................................................		499
13.26	End Point Error Check Cancellation; G69.......................................................................		502
13.27	Coordinate Read Function; G14 .....................................................................................		504

14. Coordinates System Setting Functions................................................................................		507
14.1	Coordinate Words and Control Axes.................................................................................	507
14.2	Basic Machine, Workpiece and Local Coordinate Systems..............................................	508
14.3	Machine Zero Point and 2nd, 3rd, 4th Reference Positions..............................................	509
14.4	Basic Machine Coordinate System Selection; G53...........................................................	510

14.5	Coordinate System Setting; G92.......................................................................................		511
14.6	Automatic Coordinate System Setting ..............................................................................		512
14.7	Reference (Zero) Position Return; G28, G29....................................................................		513
14.8	2nd, 3rd and 4th Reference (Zero) Position Return; G30 .................................................		517
14.9	Reference Position Check; G27........................................................................................		520
14.10 Workpiece Coordinate System Setting and Offset ; G54 to G59 (G54.1) .......................			521
14.11 Local Coordinate System Setting; G52 ...........................................................................			533
14.12 Workpiece Coordinate System Preset; G92.1 ................................................................			537
14.13 Coordinate System for Rotary Axis .................................................................................			542
15. Measurement Support Functions..........................................................................................			545
15.1	Automatic Tool Length Measurement; G37.1 ...................................................................		545
15.2	Skip Function; G31............................................................................................................		549
15.3	Multi-step Skip Function; G31.n, G04 ...............................................................................		554
15.4	Multi-step Skip Function 2; G31 ........................................................................................		556
15.5	Speed Change Skip; G31 .................................................................................................		558
15.6	Programmable Current Limitation .....................................................................................		561
15.7	Stroke Check Before Travel; G22.1/G23.1 .......................................................................		562
Appendix 1.		Program Error .......................................................................................................	564
Appendix 2.		Order of G Function Command Priority..............................................................	584

1. Control Axes

1.1 Coordinate Words and Control Axis

1. Control Axes

1.1 Coordinate Words and Control Axis

Function and purpose

In the standard specifications, there are 3 control axes, but, by adding an additional axis, up to 4 axes can be controlled.

The designation of the processing direction responds to those axes and uses a coordinate word made up of alphabet characters that have been decided beforehand.

X-Y table

	+Z
+Z
+Y
+X
Program coordinates
Workpiece
X-Y table	+X

+Y	Bed Direction of
Direction of
table movement	table movement

	X-Y and revolving table
	+X		Workpiece
	Direction of table		+C
	movement	+Y
			Direction of table
			revolution

+Z

+Y +C

+X

Program coordinates

1

1. Control Axes

1.2Coordinate Systems and Coordinate Zero Point Symbols

1.2Coordinate Systems and Coordinate Zero Point Symbols

Function and purpose

: Reference position

: Machine coordinate zero point

: Workpiece coordinate zero points (G54 - G59)

-X				Machine
	Basic machine coordinate system			zero point
				x1
				y1
y3	y2			1st reference
Workpiece	Workpiece	Workpiece
				position
coordinate	coordinate	coordinate
system 3 (G56)	system 2 (G55)	system 1 (G54)
	x3	x2
			Local
			coordinate
	y5	x	system
Workpiece	Workpiece	Workpiece	(G52)	-Y
		coordinate	y
coordinate	coordinate	system 4
system 6 (G59)	system 5 (G58)	(G57)
		x5

2

2. Least Command Increments

2.1 Input Setting Units

2. Least Command Increments

2.1 Input Setting Units

Function and purpose

The input setting units are, as with the compensation amounts, the units of setting data used in common for all axes.

The command units are the movement amounts in the program which are commanded with MDI inputs or command tape. 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.

	Parameters		Linear axis			Rotation axis
			Millimeter		Inch	(°)
	#1003 iunit	= B	0.001		0.0001	0.001
Input setting unit		= C	0.0001		0.00001	0.0001
		= D	0.00001		0.000001	0.00001
		= E	0.000001		0.0000001	0.000001
	#1015 cunit	= 0		Follow #1003 iunit
		= 1	0.0001		0.00001	0.0001
Command unit		= 10	0.001		0.0001	0.001
		= 100	0.01		0.001	0.01
		= 1000	0.1		0.01	0.1
		= 10000	1.0		0.1	1.0

(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.)

3

2. Least Command Increments

2.1 Input Setting Units

Detailed description

(1)Units of various data

These input setting units determine the parameter setting unit, program command unit and the external interface unit for the PLC axis and handle pulse, etc. The following rules show how the unit of each data changes when the input setting unit is changed. This table applies to the NC axis and PLC axis.

	Data	Unit	Setting value		Input setting unit
		system		1µm (B)	0.1µm (C)	10nm (D)	1nm (E)
	Speed data	Milli-	20000 (mm/min)	20000	20000	20000	20000
		metre	Setting range	1 to 999999	1 to 999999	1 to 999999	1 to 999999
	Example:
		Inch	2000 (inch/min)	2000	2000	2000	2000
	rapid
			Setting range	1 to 999999	1 to 999999	1 to 999999	1 to 999999
	Position data	Milli-	123.123 (mm)	123.123	123.1230	123.12300	123.123000
		metre	Setting range	±99999.999	±99999.9999	±99999.99999	±99999.999999
	Example:
		Inch	12.1234 (inch)	12.1234	12.12340	12.123400	12.1234000
	SoftLimit+
			Setting range	±9999.9999	±9999.99999	±9999.999999	±9999.9999999
		Milli-	1 (µm)	2	20	200	2000
	Interpolation	metre	Setting range	±9999	±9999	±9999	±9999
	unit data	Inch	0.001 (inch)	2	20	200	2000
			Setting range	±9999	±9999	±9999	±9999

(2)Program command

The program command unit follows the above table.

If the data has a decimal point, the number of digits in the integer section will remain and the number of digits in the decimal point section will increase as the input setting unit becomes smaller.

When setting data with no decimal point, and which is a position command, the data will be affected by the input setting increment and input command increment.

For the feed rate, as the input setting unit becomes smaller, the number of digits in the integer section will remain the same, but the number of digits in the decimal point section will increase.

4

2. Least Command Increments

2.2 Input Command Increment Tenfold

2.2 Input Command Increment Tenfold

Function and purpose

The program's command increment can be multiplied by an arbitrary scale with the parameter designation.

This function is valid when a decimal point is not used for the command increment. The scale is set with the parameters.

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			"UNIT*10" parameter
	(Machining program:
	programmed with 1=10µm)
					10		1
	(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

-300	-200		-100
			N1	W
			N2	-100
		N3
N4				-200
	N5			-300
R		N6
				-400

UNIT*10 ON

-30	-20	-10
		N1	W
		N2	-10
		N3
	N4		-20
		N6	-30
	N5
	R
			-40

UNIT*10 OFF

5

2. Least Command Increments

2.3 Indexing Increment

2.3 Indexing Increment

Function and purpose

This function limits the command value for the rotary axis.

This can be used for indexing the rotary table, etc. It is possible to cause a program error with a program command other than an indexing increment (parameter setting value).

Detailed description

When the indexing increment (parameter) for limiting the command value is set, the rotary axis can be positioned with that indexing increment. If a program other than the indexing increment setting value is commanded, a program error (P20) will occur.

The indexing position will not be checked when the parameter is set to 0.

(Example) When the indexing increment setting value is 2 degrees, only command with the 2-degree increment are possible.

G90 G01 C102. 000 ; … Moves to the 102 degree angle.

G90 G01 C101. 000 : … Program error

G90 G01 C102 ; … Moves to the 102 degree angle. (Decimal point type II)

The following axis specification parameter is used.

	#	Item	Contents	Setting range
				(unit)
	2106	Index unit Indexing	Set the indexing increment to which the rotary	0 to 360 (° )
		increment	axis can be positioned.

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.

6

3. Data Formats

3.1 Tape Codes

3. Data Formats

3.1 Tape Codes

Function and purpose

The tape command codes used for this controller are combinations of alphabet letters (A, B, C, ...

Z), numbers (0, 1, 2 ... 9) and signs (+, -, / ...). These alphabet letters, numbers and signs are referred to as characters. Each character is represented by a combination of 8 holes which may, or may not, be present.

These combinations make up what is called codes. This controller uses, the ISO code (R-840).

(Note 1) If a code not given in the tape code table in Fig. 1 is assigned during operation, program error (P32) will result.

(Note 2) For the sake of convenience, a semicolon " ; " has been used in the CNC display to indicate the end of a block (EOB/IF) which separates one block from another. Do not use the semicolon key, however, in actual programming but use the keys in the following table instead.

CAUTION

“EOB", "%", and “EOR” are symbols used for explanation. The actual codes for ISO are "CR, LF" ("LF") and "%".

The programs created on the Edit screen are stored in the NC memory in a "CR, LF" format, however, the programs created with external devices such as the FLD or RS-232C may be stored in an "LF" format.

The actual codes for EIA are "EOB (End of Block)" and "EOR (End of Record)".

Detailed description

EOB/EOR keys and displays

	Code used	ISO	Screen display
	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.

7

3. Data Formats

3.1 Tape Codes

(2)Control out, control in

All data between control out "(" and control in ")" or ";" , from "0" to ";" (when label L) are ignored, although these data appear on the setting and display unit. Consequently, the command tape name, No. 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

FL CRG 0 0 X - 8 5 0 0 0 Y - 6 4 0 0 0 ( CUT T ERSPRE T URN ) FL

•

•

••

•

•

••

•

••

•

•

•

•

•

• ••

•

••

•• •• •

•

•

•

••••

•• •

••

••

•••

•

•••

• ••

• • • • • • • • • ••• • •

••••

• • •

••

• • • • •

• • • • • • • • • • • • •••••• •

•••••

•••

•••

••••••

•••••

••• •

•

•••

••

••••••

••••

•••

•

••••••

••••••••

••••••

•

•••••••

•

• ••

•

•

•

•

•

•••••••

• • • •

Operator information print-out example

Information in this section is ignored and nothing is executed.

The difference of the label and variable code is the following tables.

Code	Control in/out range	Label (L)	Label (O)
ISO/EIA	Form "(" to ")"	Ignore the data.	Ignore the data.
	From "O" to "; (EOB)"	Ignore the data.	The value after "O" will be
			handled as label No.

(Note) Always set "O" at the head of the block. A program error (P32) will occur if there is "O" besides the head of the block.

(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 ;		• • • • • • • •	;	• • • • • •	;	• • • • • • • • • •	;	10cm	%
(EOR)	(EOB)	(EOB)			(EOB)	(EOB)		(EOR)
2m		Initial block				Last block			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.

8

3. Data Formats

3.1 Tape Codes

ISO code (R-840)

Feed holes

8 7 6 5 4 3 2 1

•	•		•		•	•
•	•		•
•	•		•	•	••
	•		•			•
	•		•	•
•	•		•	••
	•		•	•••
•	••		•			•
•	••		•
	•		••		•	•
•			•
••			•	•	••
•			•			•
••			•	•
••			•	••
•		•	•	•••
•			•			•
••		•	•		•
••		•	•
•		•	•	•	••
••		•	•			•
•		•	•	•
•		•	•	••
••	•	•	•	•••
•			•			•
••	•		•		•
••	•		•
•	•		•	•	••
••	•		•			•
•	•		•	•
•	•		•	••
••	•		•	•••
••	••		•			•
•	••		•		•
•	••		•
		•	•	•	••
		•	•			•
•		•	•	••
		•	•	•
•		•	•	•••
•		•	•	•	•	•
		•	•
•		•	•			•
		•	•		•
•	••		•
		•	•		••
•			•	•	•	•
•	••		•
••	••		•	•	••
••	••		•			•
•		•	•	•		•
•			•
•		•	•	•••
•		•	••
			••	•		•
•	••		•	•••
			•	•	••
•	••		•
	••		•	••
••	••		•	•••
	••		••		•
••			•	•••
••	••		•	•••
			•
			•
			•

Channel No.

1
2
3
4
5
6
7
8
9
0
A
B
C
D
E
F
G
H
I
J
K
L
M
N
O
P
Q
R
S
T
U
V
W
X
Y
Z
+
-
.
,
/
%
LF(Line Feed) or NL
( (Control Out)
) (Control In)
:
#
*
=
[
]
SP(Space)
CR(Carriage Return)
BS(Back Space)
HT(Horizontal Tab)
&
!
$
' (Apostrophe)	A
;
<
>
?
@
"
DEL(Delete)	B
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.

Code A are stored on tape but an error results (except when they are used in the comment section) during operation.

The B codes are non-working codes and are always ignored. Parity V check is not executed.

Table of tape codes

9

3. Data Formats

3.2 Program Formats

3.2 Program Formats

Function and purpose

The prescribed arrangement used when assigning control information to the controller is known as the program format, and the format used with this controller is called the "word address format".

Detailed description

(1)Word and address

A word is a collection of characters arranged in a specific sequence. 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.).

Word

*

Numerals

Alphabet (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

2 blocks

Since the semicolon in the parentheses will not result in an EOB, it is 1 block.

A program is a collection of several blocks.

10

3. Data Formats

					3.2	Program Formats
<Brief summary of format details>					Rotary axis
			Metric command	Inch command		Rotary axis
					(Metric command)	(Inch command)
Program No.			L(O)8	←	←	←
Sequence No.			N6	←	←	←
Preparatory function			G3/G21	←	←	←
		0.001(°) mm/	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
		0.001 inch
		0.0001(°) mm/	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
Movement		0.0001 inch
axis		0.00001(°) mm/	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
		0.00001 inch
		0.000001(°) mm/	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
		0.000001 inch
		0.001(°) mm/	I+53 J+53 K+53	I+44 J+44 K+44	I+53 J+53 K+53	I+53 J+53 K+53
		0.001 inch				(Note 5)
Arc and		0.0001(°) mm/	I+54 J+54 K+54	I+45 J+45 K+45	I+54 J+54 K+54	I+54 J+54 K+54
		0.0001 inch				(Note 5)
cutter
		0.00001(°) mm/				I+55 J+55 K+55
radius			I+55 J+55 K+55	I+46 J+46 K+46	I+55 J+55 K+55
		0.00001 inch				(Note 5)
		0.000001(°) mm/	I+56 J+56 K+56	I+47 J+47 K+47	I+56 J+56 K+56	I+56 J+56 K+56
		0.000001 inch				(Note 5)
Dwell		0.001(rev)/(s)	X53/P8	←	←	←
		0.001(°) mm/	F63	F54	F63	F54 (Note 6)
		0.001 inch
Feed
		0.0001 (°) mm/	F64	F55	F64	F55 (Note 6)
function		0.0001 inch
(Feed per		0.00001 (°) mm/	F65	F56	F65	F56 (Note 6)
minute)		0.00001 inch
		0.000001 (°) mm/	F66	F57	F66	F57 (Note 6)
		0.000001 inch
		0.0001(°) mm/	F33	F34	F33	F34 (Note 6)
		0.0001 inch
Feed
		0.00001 (°) mm/	F34	F35	F34	F35 (Note 6)
function		0.00001 inch
(Feed per		0.000001 (°) mm/	F35	F36	F35	F36 (Note 6)
revolution)		0.000001 inch
		0.0000001 (°) mm/	F36	F37	F36	F37 (Note 6)
		0.0000001 inch
Tool compensation			H3 D3	←	←	←
Miscellaneous function (M)			M8	←	←	←
Spindle function (S)			S8	←	←	←
Tool function (T)			T8	←	←	←
2nd miscellaneous function			A8/B8/C8	←	←	←
Subprogram			P8 H5 L4	←	←	←
		0.001(°) mm/	R+53 Q53 P8 L4	R+44 Q44 P8 L4	R+53 Q53 P8 L4	R+53 Q53 P8 L4
		0.001 inch
		0.0001(°) mm/	R+54 Q54 P8 L4	R+45 Q45 P8 L4	R+54 Q54 P8 L4	R+54 Q54 P8 L4
Fixed		0.0001 inch
cycle		0.00001(°) mm/	R+55 Q55 P8 L4	R+46 Q46 P8 L4	R+55 Q55 P8 L4	R+55 Q55 P8 L4
		0.00001 inch
		0.000001(°) mm/	R+56 Q56 P8 L4	R+47 Q47 P8 L4	R+56 Q56 P8 L4	R+56 Q56 P8 L4
		0.000001 inch

(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	: L(O)8 :8-digit program No.
Example 2	: G21 :Dimension G is 2 digits to the left of the decimal point, and 1 digit to the right.
Example 3	: X+53 :Dimension X uses + or - sign and represents 5 digits to the left of the decimal
	point and 3 digits to the right.
	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.

(Note 10) The addresses of the program No. and subprogram call No. differ according to the parameter. The system must be formatted when this parameter is changed.

Setting of	Address of the	Address to call the
“#11009 M2 labelO”	program No.	subprogram
0	L	L
1	O	A

This manual describes on the assumption that the parameter is set to "0".

12

3. Data Formats

3.3 Tape Memory Format

3.3 Tape Memory Format

Function and purpose

(1)Storage tape and significant sections

The others are about from the current tape position to the EOB. Accordingly, under normal conditions, operate the tape memory after resetting.

The significant codes listed in "Table of tape codes" 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.

3.4Optional Block Skip

3.4.1 Optional Block Skip ; /

Function and purpose

This function selectively ignores specific blocks in a machining program which starts with the "/" (slash) code.

Detailed description

(1)Provided that the optional block skip switch is ON, blocks starting with the "/" code are ignored. They are executed if the switch is OFF.

Parity check is valid regardless of whether the optional block skip switch is ON or OFF. When, for instance, all blocks are to be executed for one workpiece but specific block are not to be executed for another workpiece, the same command tape can be used to machine different parts by inserting the "/" code at the head of those specific blocks.

Precautions for using optional block skip

(1)Put the "/" code for optional block skip at the beginning of a block. If it is placed inside the block, it is assumed as a user macro, a division instruction.

Example : N20 G1 X25./Y25. ;....NG (User macro, a division instruction; a program error results.)

/N20 G1 X25. Y25. ;.....OK

(2)Parity checks (H and V) are conducted regardless of the optional block skip switch position.

(3)The optional block skip is processed immediately before the pre-read buffer.

Consequently, it is not possible to skip up to the block which has been read into the pre-read buffer.

(4)This function is valid even during a sequence number search.

(5)All blocks with the "/" code are also input and output during tape storing and tape output, regardless of the position of the optional block skip switch.

13

3. Data Formats

3.4 Optional Block Skip

3.4.2 Optional Block Skip Addition ; /n

Function and purpose

Whether the block with "/n (n:1 to 9)" (slash) is executed during automatic operation and searching is selected.

By using the machining program with "/n" code, different parts can be machined by the same program.

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		Part 2
the optional block skip 5 signal ON		the optional block skip 5 signal OFF
N4	N2	N4	N3	N2

14

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;	(a) Optional block skip 1 signal ON
/1/2		N02	G00	X50.;	(Optional block skip 2, 3 signals OFF)
/1/2		N03	G01	Z-20. F100;	N01 -> N08 -> N09 -> N10 -> N11 -> N12
/1/2		N04	G00	Z3.;
/1	/3	N05	G00	X30.;	(b) Optional block skip 2 signal ON
/1	/3	N06	G01	Z-20. F100;	(Optional block skip 1, 3 signals OFF)
/1 /3		N07	G00	Z3.;	N01 -> N05 -> N06 -> N07 -> N11 -> N12
/2/3		N08	G00	X10.;
/2/3		N09	G01	Z-20. F100;	(c) Optional block skip 3 signal ON
/2/3		N10	G00	Z3.;	(Optional block skip 1, 2 signals OFF)
		N11 G28 X0 M05;			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

3.5Program/Sequence/Block Numbers ; L(O), N

3.5Program/Sequence/Block Numbers ; L(O), N

Function and purpose

These numbers are used for monitoring the execution of the machining programs and for calling both machining programs and specific stages in machining programs.

(1)Program numbers are classified by workpiece correspondence or by subprogram units, and they are designated by the address "L" (or "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		Monitor display
		Program No.	Sequence No.	Block No.
	L12345678 (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
	%

16