MITSUBISHI CNC M700L, M700LV, M70L Programming Manual

MELDAS is a registered trademark of Mitsubishi Electric Corporation.

Other brands and product names throughout this manual are trademarks or registered trademarks of their respective holders.

Introduction

This instruction manual describes the methods of using the MITSUBISHI CNC MULTI-AXIS,MULTI-PART SYSTEM M700L/M700LV/M70L Series mainly for a lathe.

The programming methods for all of the above models are described, so read this manual thoroughly before starting use.

In respect to the functions related to the multi-axis multi-part system, the programming and alarm details for each system are the same as the general-purpose (2-axis, 3-axis) lathe. Explanations in this manual assume that all functions are provided with all of the above models. However, all options are not necessarily provided with each CNC, so refer to the specifications issued by the machine manufacturer before starting use.

Thoroughly read the "Precautions for Safety" given on the next page to ensure safe use of this numerical control unit.

Details described in this manual

(1)This manual gives general explanations from the standpoint of the NC side.

For explanations concerning individual machine tools, refer to the instruction manual issued by the machine manufacturer.

For items described as "Restrictions, "Usable State", etc., the instruction manual issued by the machine manufacturer takes precedence over this manual.

(2)While every effort has been made to describe special handling in this manual, items not described in this manual should be interpreted as "Not Possible".

(3)The multi-part system function is an additional specification. The 3-system model is explained as an example in this manual, but the number of systems that can be used will differ according to the model.

Note that the maximum number of spindle axes will also differ according to the model. Check the specifications before starting use.

(4)Some functions are unavailable depending on the machine model.

CAUTION

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

Items not described in this instruction manual should be interpreted as "Not Possible".

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

Refer to the instruction manual issued by the machine manufacturer for explanations on each machine tool.

Some screens and functions may differ or may not be usable depending on the NC system version.

Precautions for Safety

Always read the specifications issued by the machine maker, this manual, related manuals and attached documents before installation, operation, programming, maintenance or inspection to ensure correct use.

Understand this numerical controller, safety items and cautions before using the unit. This manual ranks the safety precautions into "DANGER", "WARNING" and "CAUTION".

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

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

DANGER

Not applicable in this manual.

WARNING

Not applicable in this manual.

CAUTION

1. Items related to product and manual

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

Items not described in this instruction manual should be interpreted as "Not Possible".

This manual is written on the assumption that all option functions are added. Refer to the specifications issued by the machine manufacturer before starting use.

Some screens and functions may differ or may not be usable depending on the NC system version.

CAUTION

2. Items related to programming

Because of key chattering etc., during editing, the commands with no value after G become a "G00" operation during running.

";", "EOB" and "%" "EOR" are expressions used for the explanation. The actual codes are "; (line feed)" and "%" for ISO, and "EOB" (End Of Block) and "EOR" (End Of Record) for EIA.

The commands with no value after G become a "G00" operation during running.

Always carry out dry run operation before actual machining, and confirm the machining program, tool offset amount and workpiece offset amount, etc.

When creating the machining program, select adequate machining conditions, and make sure not to exceed the machine and NC's performance, capacity and limits. Examples given in this manual do not take the machining conditions into consideration.

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

When programming the multi-part system, take special care to the movements of the programs for other systems.

During the spindle synchronous control mode, do not turn the rotation command for the slave spindle OFF while the master spindle and slave spindle are chucked on the same workpiece. This will be hazardous as the slave spindle will stop.

Do not issue another axis name change command before axis name change cancel is issued once axis name change is commanded.

Disposal

(Note) This symbol mark is for EU countries only.

This symbol mark is according to the directive 2006/66/EC Article 20 Information for endusers and Annex II.

Your MITSUBISHI ELECTRIC product is designed and manufactured with high quality materials and components which can be recycled and/or reused.

This symbol means that batteries and accumulators, at their end-of-life, should be disposed of separately from your household waste.

If a chemical symbol is printed beneath the symbol shown above, this chemical symbol means that the battery or accumulator contains a heavy metal at a certain concentration. This will be indicated as follows:

Hg: mercury (0,0005%), Cd: cadmium (0,002%), Pb: lead (0,004%)

In the European Union there are separate collection systems for used batteries and accumulators. Please, dispose of batteries and accumulators correctly at your local community waste collection/ recycling centre.

Please, help us to conserve the environment we live in!

Contents

1. CONTROL AXES............................................................................................................................			1
1.1	Coordinate Word and Control Axis..........................................................................................		1
1.2	Coordinate Systems and Coordinate Zero Point Symbols......................................................		2
2. INPUT COMMAND UNITS .............................................................................................................			3
2.1	Input Command Units .............................................................................................................		3
2.2	Input Setting Units...................................................................................................................		3
3. DATA FORMATS ...........................................................................................................................			4
3.1	Tape Codes.............................................................................................................................		4
3.2	Program Formats ....................................................................................................................		6
3.3	Tape Storage Format ..............................................................................................................		8
3.4	Optional Block Skip .................................................................................................................		8
3.5	Program/Sequence/Block Numbers (O, N) .............................................................................		9
3.6	G Code System.....................................................................................................................		10
3.7	Precautions Before Machining ..............................................................................................		14
4. BUFFER REGISTER ....................................................................................................................			15
4.1	Pre-read Buffers....................................................................................................................		15
5. POSITION COMMANDS ..............................................................................................................			16
5.1	Incremental/Absolute Value Commands...............................................................................		16
5.2	Radius/Diameter Commands ................................................................................................		18
5.3	Inch/Metric Conversion (G20, G21) ......................................................................................		19
5.4	Decimal Point Input ...............................................................................................................		20
6. INTERPOLATION FUNCTIONS...................................................................................................			24
6.1	Positioning (Rapid Traverse); G00........................................................................................		24
6.2	Linear Interpolation; G01.......................................................................................................		27
6.3	Circular Interpolation; G02, G03 ...........................................................................................		29
6.4	R-designated Circular Interpolation; G02, G03 .....................................................................		33
6.5	Plane Selection; G17, G18, G19...........................................................................................		35
6.6	Helical interpolation; G17, G18, G19, and G02, G03............................................................		37
6.7	Thread Cutting ......................................................................................................................		41
6.7.1 Constant lead thread cutting; G33 ..................................................................................			41
6.7.2 Inch thread cutting; G33 .................................................................................................			45
6.7.3		Continuous thread cutting...............................................................................................	46
6.7.4 Variable lead thread cutting ............................................................................................			47
6.7.5 Circular thread cutting; G35/G36 ....................................................................................			49
6.8	Milling Interpolation; G12.1/G13.1.........................................................................................		55
6.8.1		Selecting milling mode....................................................................................................	56
6.8.2 Milling interpolation control and command axes.............................................................			57
6.8.3 Selecting a plane during the milling mode ......................................................................			59
6.8.4 Setting milling coordinate system ...................................................................................			61
6.8.5		Preparatory functions......................................................................................................	63
6.8.6 Switching from milling mode to turning mode; G13.1 .....................................................			68
6.8.7		Feed function ..................................................................................................................	68
6.8.8		Program support functions..............................................................................................	68
6.8.9		Miscellaneous functions..................................................................................................	69
6.8.10		Tool offset functions......................................................................................................	70
6.8.11		Interference check ........................................................................................................	87
7. FEED FUNCTIONS.......................................................................................................................			95
7.1	Rapid Traverse Rate .............................................................................................................		95
7.2	Cutting Feedrate ...................................................................................................................		95

7.3	Synchronous/Asynchronous Feed; G94, G95.......................................................................			96
7.4	Feedrate Designation and Effects on Control Axes ..............................................................			98
7.5		Thread Cutting Leads..........................................................................................................		102
7.6		Automatic Acceleration/Deceleration ..................................................................................		103
7.7	Rapid Traverse Constant Inclination Acceleration/Deceleration .........................................			104
7.8		Speed Clamp ......................................................................................................................		106
7.9	Exact Stop Check; G09.......................................................................................................			107
7.10		Exact Stop Check Mode; G61...........................................................................................		111
7.11		Cutting Mode; G64 ............................................................................................................		111
7.12		Feed Forward Control .......................................................................................................		112
8. DWELL			.......................................................................................................................................	113
8.1	Dwell Per Second; (G94) G04.............................................................................................			113
8.2	Dwell ...........................................................................................Per Rotation; (G95) G04			115
9. MISCELLANEOUS ...............................................................................................FUNCTIONS				116
9.1	Miscellaneous ............................................................................Functions (M2-digit BCD)			116
9.2		Miscellaneous .....................................................................................Functions (M8-digit)		118
9.3	2nd ...................................................................Miscellaneous Functions (A8/B8/C8-digit)			118
10. SPINDLE .............................................................................................................FUNCTIONS				119
10.1		Spindle .....................................................................................Functions (S2-digit BCD)		119
10.2		Spindle ..............................................................................................Functions (S8-digit)		119
10.3		Constant .....................................................................Surface Speed Control; G96, G97		120
10.4		Spindle ..................................................................................Clamp Speed Setting; G92		127
10.5		Spindle ...............................................................................Functions (Multiple Spindles)		129
10.5.1 ........................................................................................			Multiple - spindle commands	130
10.6		Second ......................................................................................Spindle Control Function		132
10.6.1 ............................................................................Second spindle extension selection				134
11. TOOL ..................................................................................................................FUNCTIONS				135
11.1		Tool ...................................................................................................Functions (T4-digit)		135
11.2		Tool ...................................................................................................Functions (T8-digit)		136
11.3		Number ...........................................................of T Command Digits Judgment Function		137
12. TOOL ...................................................................................................OFFSET FUNCTIONS				139
12.1		Tool .........................................................................................................................Offset		139
12.2		Tool .............................................................................................................Length Offset		141
12.3		Tool ......................................................................................................Nose Wear Offset		143
12.3.1 .............................................................................................Wear offset amount hold				144
12.4		Nose ...................................................................R Compensation; G40, G41, G42, G46		145
12.4.1 ............................................................Tool nose point and compensation directions				147
12.4.2 ...............................................................................Nose R compensation operations				150
12.4.3 ..........................................................Other operations during nose R compensation				160
12.4.4 ..............................................................G41/G42 commands and I, J, K designation				168
12.4.5 ......................................................................Interrupts during nose R compensation				173
12.4.6 ...........................................................General precautions for nose R compensation				176
12.4.7 ......................................................................................................			Interference check	177
12.5		Programmed .................................................................................Tool Offset Input; G10		182
12.6		Common ....................................................................................................System Offset		185
13. PROGRAM .......................................................................................SUPPORT FUNCTIONS				186
13.1		Fixed ...................................................................................................Cycles for Turning		186
13.1.1 ...................................................................................Longitudinal cutting cycle; G77				187
13.1.2 ...........................................................................................Thread cutting cycle; G78				189
13.1.3 ..............................................................................................Face cutting cycle; G79				192
13.2		Compound ...................................................................................................Fixed Cycles		195

13.2.1 Longitudinal rough cutting cycle I; G71.......................................................................			196
13.2.2 Face rough cutting cycle I; G72 ..................................................................................			201
13.2.3 Formed material rough cutting cycle; G73 ..................................................................			206
13.2.4		Finishing cycle; G70 ...................................................................................................	210
13.2.5 Face cut-off cycle; G74...............................................................................................			211
13.2.6 Longitudinal cut-off cycle; G75 ...................................................................................			213
13.2.7 Compound thread cutting cycle; G76..........................................................................			215
13.2.8 Precautions for compound fixed cycles (G70 to G76) ................................................			219
13.3 Hole Drilling Fixed Cycles; G80 to G89.............................................................................			221
13.3.1 G83 face deep hole drilling cycle 1 (G87 longitudinal deep hole drilling cycle 1) .......			225
13.3.2 G84 face tapping cycle (G88 longitudinal tapping cycle)............................................			227
13.3.3 G85 face boring cycle (G89 longitudinal boring cycle)................................................			232
13.3.4 G80 hole drilling fixed cycle cancel.............................................................................			232
13.3.5 Precautions for using hole drilling fixed cycles ...........................................................			233
13.4 Deep Hole Drilling Cycle 2; G83.2 ....................................................................................			234
13.5 Subprogram Control; M98, M99........................................................................................			237
13.6	Variable Commands..........................................................................................................		243
13.7	User Macro........................................................................................................................		245
13.7.1 User macro commands; G65, G66, G66.1, G67.........................................................			245
13.7.2		Macro call instruction ..................................................................................................	246
13.7.3 G code for macro ........................................................................................................			253
13.7.4		Variables.....................................................................................................................	254
13.7.5		Types of variables.......................................................................................................	256
13.7.6		Operation commands..................................................................................................	271
13.7.7		Control commands......................................................................................................	276
13.7.8		Precautions.................................................................................................................	279
13.8 Double-Turret Mirror Image; G68, G69 .............................................................................			281
13.9 Corner Chamfering, Corner Rounding Function I .............................................................			286
13.9.1		Corner chamfering (,C_ ) ............................................................................................	286
13.9.2		Corner rounding (,R_ )................................................................................................	288
13.10 Corner Chamfering, Corner Rounding Function II ..........................................................			290
13.10.1		Corner chamfering (,C_) ...........................................................................................	290
13.10.2		Corner rounding (,R_ )..............................................................................................	292
13.10.3 Interrupt during corner chamfering/rounding.............................................................			294
13.11	Linear Angle Command ..................................................................................................		295
13.12	Geometric Command ......................................................................................................		296
13.12.1		Geometric command IA ............................................................................................	296
13.13 Program Parameter Input; G10/G11 ...............................................................................			299
13.14	Programmable In-position Check....................................................................................		307

13.15Positioning (G00)/Machine Coordinate System Selection (G53) Feedrate

	Designation.....................................................................................................................	310
13.16 Inclined Coordinate Rotation; G173 ................................................................................		316
14. COORDINATE SYSTEM SETTING FUNCTIONS....................................................................		328
14.1	Coordinate Words and Control Axes.................................................................................	328
14.2	Basic Machine, Workpiece and Local Coordinate Systems..............................................	329
14.3	Machine Zero Point and 2nd Reference Point (Zero Point) ..............................................	330
14.4	Automatic Coordinate System Setting ..............................................................................	331
14.5	Machine Coordinate System Selection; G53 ....................................................................	332
14.6	Coordinate System Setting; G92.......................................................................................	333
14.7	Reference Point Return; G28, G29 ...................................................................................	334
14.8	2nd, 3rd, and 4th Reference (Zero) Point Return; G30.....................................................	338
14.9	Reference Point Check; G27 ............................................................................................	341
14.10 Workpiece Coordinate System Setting and Offset; G54 to G59 .....................................		342

14.11 Local Coordinate System Setting; G52 ...........................................................................				347
15. PROTECTION FUNCTIONS.....................................................................................................				348
15.1	Chuck Barriers/Tailstock Barriers......................................................................................			348
16. MEASUREMENT SUPPORT FUNCTIONS..............................................................................				351
16.1	Skip Function; G31............................................................................................................			351
16.2	Multi-step Skip Function; G31 ...........................................................................................			356
16.3	Automatic Tool Length Measurement; G37 ......................................................................			358
17. MULTI-AXIS, MULTI-PART SYSTEM COMPOUND CONTROL FUNCTIONS.......................				361
17.1	Synchronizing Operation between Systems .....................................................................			364
17.2	Start Point Designation Synchronizing (Type 1); G115.....................................................			369
17.3	Start Point Designation Synchronizing (Type 2); G116.....................................................			371
17.4	Balance Cut Command; G15, G14 ...................................................................................			373
17.5	Program Call Control.........................................................................................................			376
17.6	Cross Axis Control; G110..................................................................................................			377
17.7	Control Axis Synchronization ; G125 ................................................................................			383
17.8	Spindle Synchronization; G114.1, G113 ...........................................................................			386
17.9	Tool/Spindle Synchronization 1 (Polygon); G114.2, G113................................................			393
17.10 Tool/Spindle Synchronization 2 (Hobb Machining); G114.3, G113.................................				400
17.11 Control Axis Superimposition; G126 ...............................................................................				411
17.12 Spindle Superimposition; G164, G113............................................................................				426
17.12.1 Relation with other functions.....................................................................................				430
17.12.2			Precautions and restrictions .....................................................................................	431
17.13 2-System Simultaneous Thread-cutting Cycle ................................................................				433
17.13.1			Parameter setting command.....................................................................................	433
17.13.2 2-system simultaneous thread-cutting cycle I...........................................................				434
17.13.3 2-system simultaneous thread cutting cycle II ..........................................................				436
18. OTHER MULTI-AXIS, MULTI-PART SYSTEM CONTROL FUNCTIONS................................				439
18.1	Miscellaneous Function Output during Axis Movement; G117 .........................................			439
18.2	G Code Macros .................................................................................................................			441
18.3	Axis Name Change; G111 ................................................................................................			442
APPENDIX 1 LIST OF FUNCTION CODES ................................................................................				450
APPENDIX 2 LIST OF COMMAND VALUES AND SETTING RANGES ....................................				451
APPENDIX 3 CIRCULAR CUTTING RADIUS ERROR...............................................................				452
APPENDIX 4 STANDARD FIXED CYCLE SUBPROGRAMS.....................................................				453
APPENDIX 5 LIST OF VARIABLE NUMBERS...........................................................................				461
APPENDIX 6 CORRESPONDENCE TABLE OF PROGRAM PARAMETER INPUT N NUMBERS
			...............................................................................................................................	463
6.1.1		Control parameter.........................................................................................................		464
6.1.2		Axis parameter..............................................................................................................		466
6.1.3		Setup parameter ...........................................................................................................		467
6.1.4		Setup parameter 2 ........................................................................................................		469
6.2.1		Base axis parameter.....................................................................................................		470
6.2.2		Base system parameter ................................................................................................		471
6.2.3		Base common parameter..............................................................................................		473
6.2.4		Axis specification parameter.........................................................................................		475
6.2.5 Zero point return parameter..........................................................................................				476
6.2.6		Absolute position set.....................................................................................................		477
6.2.7		Position switch ..............................................................................................................		477
6.2.8		Servo parameter ...........................................................................................................		478

6.2.9		Machine error compensation ........................................................................................	478
6.2.10		Machine compensation data.......................................................................................	478
6.2.11		Macro list ....................................................................................................................	479
6.2.12		Spindle NC parameter ................................................................................................	484
6.2.13		Spindle parameter.......................................................................................................	485
6.2.14 Spindle type servo parameter .....................................................................................			485
6.2.15		PLC constant ..............................................................................................................	486
6.2.16		PLC timer....................................................................................................................	486
6.2.17		PLC counter................................................................................................................	486
6.2.18		Bit selection ................................................................................................................	486
APPENDIX 7 SUPPLEMENTARY DETAILS ON INCOMPLETE THREAD AREAS ARISING
		DURING THREAD CUTTING................................................................................	487
APPENDIX 8 MACRO INTERFACE EXPANSION......................................................................			491
8.1	Macro Interface Input ..........................................................................................................		492
8.2	Macro Interface Output .......................................................................................................		494
APPENDIX 9 SYSTEM COMMON POSITION INFORMATION RETRIEVING VARIABLES......			496
APPENDIX 10 PROGRAM ERRORS ..........................................................................................			498

1. CONTROL AXES

1.1 Coordinate Word and Control Axis

1. CONTROL AXES

1.1Coordinate Word and Control Axis

Function and purpose

In the case of a lathe, the axis parallel to the spindle is known as the Z axis and its forward direction is the direction in which the turret moves away from the spindle stock while the axis at right angles to the Z axis is the X axis and its forward direction is the direction in which it moves away from the Z axis, as shown in the figure below.

Tailstock

Spindle stock

	Tool	+Z
+Y	Turret	+X

Coordinate axes and polarities

Since coordinates based on the right hand rule are used with a lathe, the forward direction of the Y axis in the above figure which is at right angles to the X-Z plane is downward. It should be borne in mind that an arc on the X-Z plane is expressed as clockwise or counterclockwise as seen from the forward direction of the Y axis. (Refer to the section on circular interpolation.)

Spindle nose

Machine zero point

G54	Workpiece zero points (G54 to G59)

G55

G58

G52 G59

Local coordinate system (Valid in G54 to G59)

G30

2nd reference position	+Z

G28 +X

Reference position

(+Y)

Relationship between coordinates

1

1. CONTROL AXES

1.2Coordinate Systems and Coordinate Zero Point Symbols

1.2Coordinate Systems and Coordinate Zero Point Symbols

Function and purpose

: Reference position

: Machine coordinate origin

: Workpiece coordinate zero points (G54 to G59)

Upon completion of the reference point return, the parameters are referred to and automatically set for the basic machine coordinate system and workpiece coordinate systems (G54 to G59). The basic machine coordinate system is set so that the first reference point is at the position designated by the parameter from the basic machine coordinate zero point (machine zero point).

Basic machine		Machine zero point
coordinate system				+Z
		Workpiece	Workpiece	Workpiece	Workpiece
X2	Z2	coordinate	coordinate	coordinate	coordinate	X3
		system	system	system	system6
		1 (G54)	2 (G55)	5 (G58)	(G59) Z 3
Hypothetical machine
coordinate system							Local
(shifted by G92)							coordinate
						X1	system
							(G52)
+X					Z1
					1st reference position

The local coordinate system (G52) is valid on the coordinate systems designated by the commands for the workpiece coordinate systems 1 to 6.

Using the G92 command, the basic machine coordinate system can be shifted and made the hypothetical machine coordinate system. At the same time, workpiece coordinate systems 1 to 6 are also shifted.

2

2. INPUT COMMAND UNITS

2.1 Input Command Units

2. INPUT COMMAND UNITS

2.1Input Command Units

Function and purpose

These are the units used for the movement amounts in the program as commanded by the MDI input. They are expressed in millimeters, inches or degrees (°).

2.2Input Setting Units

Function and purpose

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

The input command unit can be selected for each axis and input setting units can be selected in common for the axes by parameters from among the following types. (For further details on settings, refer to the sections about control.)

				Linear axis			Rotation
		Type	Millimeter		Inch		axis
			Diametrical	Radial	Diametrical	Radial	(°)
			command	command	command	command
	Input	#1003	0.001	0.001	0.0001	0.0001	0.001
		cunit=10
	command unit
		=1	0.0001	0.0001	0.00001	0.00001	0.0001
	Min. movement	IS-B	0.0005	0.001	0.0005	0.0001	0.001
	unit	IS-C	0.00005	0.0001	0.00005	0.00001	0.0001
	Input setting	IS-B	0.001	0.001	0.0001	0.0001	0.001
	unit	IS-C	0.0001	0.0001	0.00001	0.00001	0.0001

(Note 1) Inch/metric conversion is performed in either of 2 ways: conversion from the Parameter screen ("Initial inch": valid only when the power is turned ON) and conversion using the G command (G20 or G21).

However, when a G command is used for the conversion, the conversion applies only to the input command units and not to the input setting units.

Consequently, the tool offset amounts and other compensation amounts as well as the variable data should be preset to correspond to input setting unit.

(Note 2) The millimeter and inch systems cannot be used together.

3

3. DATA FORMATS

3.1 Tape Codes

3. DATA FORMATS

3.1Tape Codes

Function and purpose

The tape command codes used for this NC are combinations of alphabet letters (A, B, C...Z), numbers (0, 1, 2...9) and signs ( +, –, /...). These alphabet letters, numbers and signs are referred to as characters. Each character is represented by a combination of 8 holes which may, or may not, be present.

These combinations make up what is called codes. This NC employs the ISO code (R-840).

CAUTION

";", "EOB" and "%" "EOR" are expressions used for the explanation. The actual codes are "line feed" and "%" for ISO.

Detailed description

(1)For the sake of convenience, a ";" has been used in the NC display to indicate End Of Block (EOB/LF) which separates one block from another. Do not use the ";" key, however, in actual programming but use the keys in the following table instead.

EOB/EOR keys and displays

	Code used	ISO	NC display
	Key used
	End Of Block	LF or NL	;
	End Of Record	%	%

(Note 1) If a code not given in Table of tape codes is assigned during operation, an Illegal address error "P32" will result.

(Note 2) The following codes which exist with ISO can be designated by parameter:

[	(left square parenthesis)
]	(right square parenthesis)
#	(sharp sign)
	(asterisk)
=	(equals sign)

:(colon)

!(exclamation mark) = (queuing code)

$ (dollar sign) = (code designating system number)

Any codes which overlap with existing codes or codes which result in parity H cannot be designated.

4

3. DATA FORMATS

3.1 Tape Codes

(2)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 first EOB (;) code after resetting to the point where the reset command is issued.

(3)Control out, control in

When the ISO code is used, all data between control out "(" and control in ")" are ignored by the NC, although these data appear on the setting display unit. Consequently, the command tape name, number and other such data not directly related to control can be inserted in this section.

This information will also be loaded, however, during tape loading.

The system is set to the "control in" mode when the power is turned ON.

Example of ISO code

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.

(4)EOR (%) code

Generally, End Of Record is punched at both ends of the tape. It has the following functions:

(a)Rewind stop when rewinding tape (with tape handler)

(b)Rewind start during tape search (with tape handler)

(c)Completion of loading during tape loading

5

3. DATA FORMATS

3.2 Program Formats

3.2Program Formats

Function and purpose

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

Detailed description

(1)Word and address

A word is a collection of characters arranged in a specific sequence. This entity is used as the unit for processing data and for causing the NC to execute specific operations.

Each word used for the NC consists of an alphabet letter and a number of several digits (sometimes with a "+" or "–" sign placed at the head of the number).

Word

------

Numerical (word data)

Alphabet (address)

Word configuration

The alphabet letter at the head of the word is the address. It defines the meaning of the numerical information which follows it.

With the NC, "S =" can be commanded for a multiple number of spindle commands although this applies only to address S.

For details of the types of words and the number of significant digits of numbers used for this NC, refer to Table 1 Format details and abbreviations.

(2)Blocks

A block is a collection of words. It includes the information which is required for the NC to execute one specific operation. One block unit constitutes a complete command. The end of each block is marked with an EOB (End-Of-Block) code.

(3)Programs

A program is a collection of several blocks.

(Note 1) If there is no number after the alphabetic character in the actual program, the value following the alphabetic character will be handled as 0.

(Example) G28XYZ; → G28X0Y0Z0;

6

3. DATA FORMATS

			3.2	Program Formats
	Table 1 Format details and abbreviations
	Item			Abbreviation
Program number			O8
Sequence number			N5
Preparatory function			G3/G21
Movement	Input setting unit	A 0.01°, mm	X + 62	Z + 62				+ 62
command
	Input setting unit	B 0.001°, mm	X + 53	Z + 53				+ 53
	Input setting unit	C 0.0001°, mm	X + 44	Z + 44				+ 44
Movement	Input setting unit	A 0.01°, mm	I + 62	K + 62
command, circular,
	Input setting unit	B 0.001°, mm	I + 53	K + 53
cutter radius
	Input setting unit	C 0.0001°, mm	I + 44	K + 44
Dwell	Input setting unit	A 0.01°, mm	X + 53	P8
	Input setting unit	B 0.001°, mm	X + 53	P8
	Input setting unit	C 0.0001°, mm	X + 53	P8
Feed function	Input setting unit	A 0.01°, mm	F62 (feed per minute)
			F43 (feed per rotation)
	Input setting unit	B 0.001°, mm	F53 (feed per minute)
			F34 (feed per rotation)
	Input setting unit	C 0.0001°, mm	F54 (feed per minute)
			F25 (feed per rotation)
Tool offset			T1/T2
Miscellaneous function			M2/M8
Spindle function			S2/S5/S8 or S		= n
Tool function			T2/T8
2nd miscellaneous function			A8/B8/C8
Subprogram			P8H5L4
Fixed cycle	Input setting unit	A 0.01°, mm	R + 62	Q62	P8		L4
	Input setting unit	B 0.001°, mm	R + 53	Q53	P8		L4
	Input setting unit	C 0.0001°, mm	R + 44	Q44	P8		L4

(Note 1) " " denotes the A, B, C, Y, P or R.

(Note 2) The number of digits in the words is checked by the maximum number of digits in the addresses.

7

3. DATA FORMATS

3.3 Tape Storage Format

3.3Tape Storage Format

Function and purpose

(1)Storage tape and storage sections

The section which is stored into the memory extends from the character following the head EOB after resetting as far as the EOR code.

The significant codes listed in Table of tape codes in Section 3.1 are the codes in the above storage section which are actually stored into the memory. All other codes are ignored and are not stored.

The data between control out "(" and control in ")" are stored into the memory.

3.4Optional Block Skip

Function and purpose

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

Detailed description

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

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

Precautions for using optional block skip

(1)Put the "/" code at the head of the block. When inserted in a block, this is handled as a division sign.

(Example) N20G1X25./Z25.;.............	NG
	(This will be handled as 25. /0, so the error P283
	"Divided by zero" will occur.)
/N20G1X25.Z25.;.............	OK

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

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

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

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

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

8

3. DATA FORMATS

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

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

Function and purpose

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

(1)Program numbers are classified by workpiece correspondence or by subprogram units, and they are designated by the address "O" followed by a number with up to 8 digits.

(2)Sequence numbers are attached where appropriate to command blocks which configure machining programs, and they are designated by the address "N" followed by a number with up to 5 digits.

(3)Block numbers are automatically provided inside the NC itself. They are preset to "0" every time a program number or sequence number is read, and they are counted up one at a time unless program numbers or sequence numbers are commanded in blocks which are subsequently read.

Consequently, all the blocks of the machining programs given in the table below can be determined without further consideration by combinations of program numbers, sequence numbers and block numbers.

	NC input machining program	NC monitor display
		Program	Sequence		Block
		No.	No.		No.
O12345678 (DEMO.PROG);		12345678	0		0
N100 G00 G90 X120. Z100.;		12345678	100		0
G94 S1000;		12345678	100		1
N102 G71 P210 Q220 I0.2 K0.2 D0.5 F600;		12345678	102		0
N200 G94 S1200 F300;		12345678	200		0
N210 G01 X0 Z95.;		12345678	210		0
G01	X20.;	12345678	210		1
G03	X50. Z80. K–15.;	12345678	210		2
G01	Z55.;	12345678	210		3
G02	X80. Z40. I15.;	12345678	210		4
G01	X100.;	12345678	210		5
G01	Z30.;	12345678	210		6
G02	Z10. K–15.;	12345678	210		7
N220 G01 Z0;		12345678	220		0
N230 G00 X120. Z150.;		12345678	230		0
N240 M02;		12345678	240		0
%		12345678	240		0

9

3. DATA FORMATS

3.6 G Code System

3.6G Code System

Function and purpose

These numbers are used to monitor the execution status of the machining program, or to call a machining program or a specific process in the machining program.

There are 3 G code systems: 1, 2 and 3. Parameters "G code type 1", "G code type 2" and "G code type 3" are used to set the applicable system.

G code system 3 is an additional specification.

The description of the G functions is based on G code system 2 which serves as the standard.

(Note 1) An alarm results when a G code not listed in the table is commanded. ("P34": Illegal G code)

(Note 2) An alarm results when a G code not included in the additional specifications is commanded.

(Example) An alarm ("P50 No spec: Inch/mm") occurs when the inch command G code (G20) is commanded although the inch/mm specifications have not been provided.

Table of G code systems

											Reference
	G code system (standard = 2)								Group	Function name	section in this
											manual
											(Section)
1				2			3
		G00			G00			G00	01	Positioning	6.1
		G01			G01			G01	01	Linear interpolation	6.2
		G02			G02			G02	01	Circular interpolation (clockwise)	6.3, 6.4
		G03			G03			G03	01	Circular interpolation (counterclockwise)	6.3, 6.4
		G04			G04			G04	00	Dwell	8.1, 8.2
		G09			G09			G09	00	Exact stop	7.8
		G10			G10			G10	00	Data setting	12.5
		G11			G11			G11	00	Data setting mode cancel	12.1
		G12.1			G12.1			G12.1	19	Milling mode ON	6.8
		G13.1			G13.1			G13.1	19	Milling mode OFF
		G14			G14			G14	18	Balance cut OFF	17.4
		G15			G15			G15	18	Balance cut ON
		G16			G16			G16	02	Y-Z cylindrical plane selection	6.8
		G17			G17			G17	02	X-Y plane selection	6.5
		G18			G18			G18	02	Z-X plane selection
		G19			G19			G19	02	Y-Z plane selection
		G20			G20			G70	06	Inch command	5.3
		G21			G21			G71	06	Metric command
		G22			G22			G22	04	Barrier check ON	15.1
		G23			G23			G23	04	Barrier check OFF

10

3. DATA FORMATS

3.6 G Code System

											Reference
	G code system (standard = 2)								Group	Function name	section in this
											manual
											(Section)
		G27			G27			G27	00	Reference point return check	14.9
		G28			G28			G28	00	Reference point return	14.7
		G29			G29			G29	00	Return from reference point
		G30			G30			G30	00	2nd reference point return	14.8
		G31			G31			G31	00	Skip function	16.1
		G32			G33			G33	01	Thread cutting	6.7
		G34			G34			G34	01	Variable lead thread cutting
		G35			G35			G35	01	Circular thread cutting (CW)
		G36			G36			G36	01	Circular thread cutting (CCW)
		G37			G37			G37	00	Automatic tool length offset, automatic tool	16.3
										length measurement
		G40			G40			G40	07	Tool nose R compensation cancel	12.4
		G41			G41			G41	07	Tool nose R compensation left
		G42			G42			G42	07	Tool nose R compensation right
		G43			G43			G43	08	2nd spindle control OFF	10.6
		G44			G44			G44	08	2nd spindle control ON
		G46			G46			G46	07	Tool nose R compensation	12.4
										(automatic selection of direction) ON
		G50			G92			G92	00	Coordinate system setting	14.6
										Spindle clamp speed setting	10.4
		G52			G52			G52	00	Local coordinate system setting	14.11
		G53			G53			G53	00	Machine coordinate system selection	14.5
		G54			G54			G54	12	Workpiece coordinate system selection 1	14.10
		G55			G55			G55	12	Workpiece coordinate system selection 2
		G56			G56			G56	12	Workpiece coordinate system selection 3
		G57			G57			G57	12	Workpiece coordinate system selection 4
		G58			G58			G58	12	Workpiece coordinate system selection 5
		G59			G59			G59	12	Workpiece coordinate system selection 6
		G61			G61			G61	13	Exact stop check mode	7.9
		G64			G64			G64	13	Cutting mode	7.10
		G65			G65			G65	00	Macro call	13.7.1
		G66			G66			G66	14	Macro modal call A
		G66.1			G66.1			G66.1	14	Macro modal call B
		G67			G67			G67	14	Macro modal call cancel
		G68			G68			G68	15	Facing turret mirror image ON	13.8
		G69			G69			G69	15	Facing turret mirror image OFF
		G70			G70			G72	09	Finishing cycle	13.2.4
		G71			G71			G73	09	Longitudinal rough cutting cycle	13.2.1
		G72			G72			G74	09	Face rough cutting cycle	13.2.2
		G73			G73			G75	09	Stock removal in rough cutting cycle	13.2.3

11

3. DATA FORMATS

3.6 G Code System

											Reference
	G code system (standard = 2)								Group	Function name	section in this
											manual
											(Section)
		G74			G74			G76	09	Face cut-off cycle	13.2.5
		G75			G75			G77	09	Longitudinal cut-off cycle	13.2.6
		G76			G76			G78	09	Compound thread cutting cycle	13.2.7
		G76.1			G76.1			G76.1	09	2-system simultaneous thread cutting cycle 1	17.13
		G76.2			G76.2			G76.2	09	2-system simultaneous thread cutting cycle 2
		G80			G80			G80	09	Hole drilling cycle cancel	13.3.4
		G83			G83			G83	09	Deep hole drilling cycle 1 (Z axis)	13.3.1
		G79			G83.2			G83.2	09	Deep hole drilling cycle 2	13.4
		G84			G84			G84	09	Tap cycle (Z axis)	13.3.2
		G85			G85			G85	09	Boring cycle (Z axis)	13.3.3
		G87			G87			G87	09	Deep hole drilling cycle (X axis)	13.3.1
		G88			G88			G88	09	Tap cycle (X axis)	13.3.2
		G89			G89			G89	09	Boring cycle (X axis)	13.3.3
		G90			G77			G20	09	Longitudinal cutting fixed cycle	13.1.1
		G92			G78			G21	09	Thread cutting fixed cycle	13.1.2
		G94			G79			G24	09	Face cutting fixed cycle	13.1.3
		G96			G96			G96	17	Constant surface speed control	10.3
		G97			G97			G97	17	Constant surface speed control cancel
		G98			G94			G94	05	Asynchronous feed	7.3
		G99			G95			G95	05	Synchronous feed
		–			G90			G90	03	Absolute value command	5.1
		–			G91			G91	03	Incremental value command
		–			G98			G98	10	Hole drilling cycle initial return	13.3
		–			G99			G99	10	Hole drilling cycle reference point return
		G110			G110			G110	00	Cross machining command	17.6
		G111			G111			G111	00	Axis name change	18.3
		G113			G113			G113	00	Spindle synchronization, tool/spindle	17.8-17.12
										synchronization cancel
		G114.1			G114.1			G114.1	00	Spindle synchronization	17.8
		G114.2			G114.2			G114.2	00	Tool/spindle synchronization 1 (polygon	17.9
										machining)
		G114.3			G114.3			G114.3	00	Tool/spindle synchronization 2 (hobb	17.10
										machining)
		G115			G115			G115	00	Waiting at designated start point 1	17.2
		G116			G116			G116	00	Waiting at designated start point 2	17.3
		G117			G117			G117	00	Miscellaneous function output during axis	18.1, 18.2
										movement
		G125			G125			G125	00	Control axis synchronization	17.7
		G126			G126			G126	00	Control axis superimposition	17.11
		G164			G164			G164	00	Spindle superimposition	17.12
		G173			G173			G173	00	Inclined coordinate rotation control	13.16
		G200 to			G200 to G999					G macro call	18.3

12

3. DATA FORMATS

3.6 G Code System

(Note 1) The " " mark denotes a G code which is selected within each group when the power is turned ON or when resetting that initializes the modal commands is executed.

(Note 2) The " " mark denotes a G code for which a parameter can be selected as the initial status when the power is turned ON or when resetting that initializes the modal commands is executed. Note that the inch/metric conversion can be made only when the power is turned ON.

CAUTION

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

13

3. DATA FORMATS

3.7 Precautions Before Machining

3.7Precautions Before Machining

Precautions before machining

CAUTION

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

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

14