fanuc 0i- F Operators Manual

FANUC Series 0+-MODEL F

For Lathe System

OPERATOR'S MANUAL

B-64604EN-1/01

•No part of this manual may be reproduced in any form.

•All specifications and designs are subject to change without notice.

The products in this manual are controlled based on Japan’s “Foreign Exchange and Foreign Trade Law”. The export of from Japan subject to an export license by the government of Japan. Other models in this manual may also be subject to export controls. Further, re-export to another country may be subject to the license of the government of the country from where the product is re-exported. Furthermore, the product may also be controlled by re-export regulations of the United States government.

Should you wish to export or re-export these products, please contact FANUC for advice.

The products in this manual are manufactured under strict quality control. However, when a serious accident or loss is predicted due to a failure of the product, pay careful attention to safety.

In this manual we have tried as much as possible to describe all the various matters. However, we cannot describe all the matters which must not be done, or which cannot be done, because there are so many possibilities.

Therefore, matters which are not especially described as possible in this manual should be regarded as “impossible”.

B-64604EN-1/01

SAFETY PRECAUTIONS

SAFETY PRECAUTIONS

This section describes the safety precautions related to the use of CNC units.

It is essential that these precautions be observed by users to ensure the safe operation of machines equipped with a CNC unit (all descriptions in this section assume this configuration). Note that some precautions are related only to specific functions, and thus may not be applicable to certain CNC units.

Users must also observe the safety precautions related to the machine, as described in the relevant manual supplied by the machine tool builder. Before attempting to operate the machine or create a program to control the operation of the machine, the operator must become fully familiar with the contents of this manual and relevant manual supplied by the machine tool builder.

CONTENTS
DEFINITION OF WARNING, CAUTION, AND NOTE.........................................................................	s-1
GENERAL WARNINGS AND CAUTIONS ............................................................................................	s-2
WARNINGS AND CAUTIONS RELATED TO PROGRAMMING.......................................................	s-3
WARNINGS AND CAUTIONS RELATED TO HANDLING ................................................................	s-5
WARNINGS RELATED TO DAILY MAINTENANCE .........................................................................	s-7

DEFINITION OF WARNING, CAUTION, AND NOTE

This manual includes safety precautions for protecting the user and preventing damage to the machine. Precautions are classified into Warning and Caution according to their bearing on safety. Also, supplementary information is described as a Note. Read the Warning, Caution, and Note thoroughly before attempting to use the machine.

WARNING

Applied when there is a danger of the user being injured or when there is a danger of both the user being injured and the equipment being damaged if the approved procedure is not observed.

CAUTION

Applied when there is a danger of the equipment being damaged, if the approved procedure is not observed.

NOTE

The Note is used to indicate supplementary information other than Warning and

Caution.

•Read this manual carefully, and store it in a safe place.

s-1

SAFETY PRECAUTIONS

B-64604EN-1/01

GENERAL WARNINGS AND CAUTIONS

WARNING

1Never attempt to machine a workpiece without first checking the operation of the machine. Before starting a production run, ensure that the machine is operating correctly by performing a trial run using, for example, the single block, feedrate override, or machine lock function or by operating the machine with neither a tool nor workpiece mounted. Failure to confirm the correct operation of the machine may result in the machine behaving unexpectedly, possibly causing damage to the workpiece and/or machine itself, or injury to the user.

2Before operating the machine, thoroughly check the entered data.

Operating the machine with incorrectly specified data may result in the machine behaving unexpectedly, possibly causing damage to the workpiece and/or machine itself, or injury to the user.

3Ensure that the specified feedrate is appropriate for the intended operation. Generally, for each machine, there is a maximum allowable feedrate.

The appropriate feedrate varies with the intended operation. Refer to the manual provided with the machine to determine the maximum allowable feedrate.

If a machine is run at other than the correct speed, it may behave unexpectedly, possibly causing damage to the workpiece and/or machine itself, or injury to the user.

4When using a tool compensation function, thoroughly check the direction and amount of compensation.

Operating the machine with incorrectly specified data may result in the machine behaving unexpectedly, possibly causing damage to the workpiece and/or machine itself, or injury to the user.

5The parameters for the CNC and PMC are factory-set. Usually, there is not need to change them. When, however, there is not alternative other than to change a parameter, ensure that you fully understand the function of the parameter before making any change.

Failure to set a parameter correctly may result in the machine behaving unexpectedly, possibly causing damage to the workpiece and/or machine itself, or injury to the user.

CAUTION

1Immediately after switching on the power, do not touch any of the keys on the

MDI unit until the position display or alarm screen appears on the CNC unit.

Some of the keys on the MDI unit are dedicated to maintenance or other special operations. Pressing any of these keys may place the CNC unit in other than its normal state. Starting the machine in this state may cause it to behave unexpectedly.

2The OPERATOR’S MANUAL and programming manual supplied with a CNC unit provide an overall description of the machine's functions, including any optional functions. Note that the optional functions will vary from one machine model to another. Therefore, some functions described in the manuals may not actually be available for a particular model. Check the specification of the machine if in doubt.

3Some functions may have been implemented at the request of the machine-tool builder. When using such functions, refer to the manual supplied by the machine-tool builder for details of their use and any related cautions.

s-2

B-64604EN-1/01

SAFETY PRECAUTIONS

CAUTION

4The liquid-crystal display is manufactured with very precise fabrication technology. Some pixels may not be turned on or may remain on. This phenomenon is a common attribute of LCDs and is not a defect.

NOTE

1Programs, parameters, and macro variables are stored in non-volatile memory in the CNC unit. Usually, they are retained even if the power is turned off.

Such data may be deleted inadvertently, however, or it may prove necessary to delete all data from non-volatile memory as part of error recovery.

To guard against the occurrence of the above, and assure quick restoration of deleted data, backup all vital data, and keep the backup copy in a safe place.

2The number of times to write machining programs to the non-volatile memory is limited.

You must use "High-speed program management" when registration and the deletion of the machining programs are frequently repeated in such case that the machining programs are automatically downloaded from a personal computer at each machining.

In "High-speed program management", the program is not saved to the non-volatile memory at registration, modification, or deletion of programs.

WARNINGS AND CAUTIONS RELATED TO PROGRAMMING

This section covers the major safety precautions related to programming. Before attempting to perform programming, read the supplied OPERATOR’S MANUAL carefully such that you are fully familiar with their contents.

WARNING

1Coordinate system setting

If a coordinate system is established incorrectly, the machine may behave unexpectedly as a result of the program issuing an otherwise valid move command. Such an unexpected operation may damage the tool, the machine itself, the workpiece, or cause injury to the user.

2Positioning by nonlinear interpolation

When performing positioning by nonlinear interpolation (positioning by nonlinear movement between the start and end points), the tool path must be carefully confirmed before performing programming. Positioning involves rapid traverse. If the tool collides with the workpiece, it may damage the tool, the machine itself, the workpiece, or cause injury to the user.

3Function involving a rotation axis

When programming polar coordinate interpolation or normal-direction

(perpendicular) control, pay careful attention to the speed of the rotation axis. Incorrect programming may result in the rotation axis speed becoming excessively high, such that centrifugal force causes the chuck to lose its grip on the workpiece if the latter is not mounted securely. Such mishap is likely to damage the tool, the machine itself, the workpiece, or cause injury to the user.

s-3

SAFETY PRECAUTIONS

B-64604EN-1/01

WARNING

4Inch/metric conversion

Switching between inch and metric inputs does not convert the measurement units of data such as the workpiece origin offset, parameter, and current position. Before starting the machine, therefore, determine which measurement units are being used. Attempting to perform an operation with invalid data specified may damage the tool, the machine itself, the workpiece, or cause injury to the user.

5Constant surface speed control

When an axis subject to constant surface speed control approaches the origin of the workpiece coordinate system, the spindle speed may become excessively high. Therefore, it is necessary to specify a maximum allowable speed. Specifying the maximum allowable speed incorrectly may damage the tool, the machine itself, the workpiece, or cause injury to the user.

6Stroke check

After switching on the power, perform a manual reference position return as required. Stroke check is not possible before manual reference position return is performed. Note that when stroke check is disabled, an alarm is not issued even if a stroke limit is exceeded, possibly damaging the tool, the machine itself, the workpiece, or causing injury to the user.

7Interference check for each path

Interference check for each path function is performed based on the tool data specified during automatic operation. If the tool specification does not match the tool actually being used, the interference check cannot be made correctly, possibly damaging the tool or the machine itself, or causing injury to the user.

After switching on the power, or after selecting a tool post manually, always start automatic operation and specify the tool number of the tool to be used.

8Same address command in same block

The G code or M code including the same address cannot be commanded on the same block. If you use the same address, it may result in the machine behaving unexpectedly, possibly causing damage to the workpiece and/or machine itself, or injury to the user. Command on separate block. About address P, refer to the appendix “List of functions include address P in the program command”

CAUTION

1Absolute/incremental mode

If a program created with absolute values is run in incremental mode, or vice versa, the machine may behave unexpectedly.

2Plane selection

If an incorrect plane is specified for circular interpolation, helical interpolation, or a canned cycle, the machine may behave unexpectedly. Refer to the descriptions of the respective functions for details.

3Torque limit skip

Before attempting a torque limit skip, apply the torque limit. If a torque limit skip is specified without the torque limit actually being applied, a move command will be executed without performing a skip.

4Programmable mirror image

Note that programmed operations vary considerably when a programmable mirror image is enabled.

s-4

B-64604EN-1/01

SAFETY PRECAUTIONS

CAUTION

5Compensation function

If a command based on the machine coordinate system or a reference position return command is issued in compensation function mode, compensation is temporarily canceled, resulting in the unexpected behavior of the machine.

Before issuing any of the above commands, therefore, always cancel compensation function mode.

WARNINGS AND CAUTIONS RELATED TO HANDLING

This section presents safety precautions related to the handling of machine tools. Before attempting to operate your machine, read the supplied OPERATOR’S MANUAL carefully, such that you are fully familiar with their contents.

WARNING

1Manual operation

When operating the machine manually, determine the current position of the tool and workpiece, and ensure that the movement axis, direction, and feedrate have been specified correctly. Incorrect operation of the machine may damage the tool, the machine itself, the workpiece, or cause injury to the operator.

2Manual reference position return

After switching on the power, perform manual reference position return as required.

If the machine is operated without first performing manual reference position return, it may behave unexpectedly. Stroke check is not possible before manual reference position return is performed.

An unexpected operation of the machine may damage the tool, the machine itself, the workpiece, or cause injury to the user.

3Manual numeric command

When issuing a manual numeric command, determine the current position of the tool and workpiece, and ensure that the movement axis, direction, and command have been specified correctly, and that the entered values are valid.

Attempting to operate the machine with an invalid command specified may damage the tool, the machine itself, the workpiece, or cause injury to the operator.

4Manual handle feed

In manual handle feed, rotating the handle with a large scale factor, such as 100, applied causes the tool and table to move rapidly. Careless handling may damage the tool and/or machine, or cause injury to the user.

5Disabled override

If override is disabled (according to the specification in a macro variable) during threading, rigid tapping, or other tapping, the speed cannot be predicted, possibly damaging the tool, the machine itself, the workpiece, or causing injury to the operator.

6Origin/preset operation

Basically, never attempt an origin/preset operation when the machine is operating under the control of a program. Otherwise, the machine may behave unexpectedly, possibly damaging the tool, the machine itself, the tool, or causing injury to the user.

s-5

SAFETY PRECAUTIONS

B-64604EN-1/01

WARNING

7Workpiece coordinate system shift

Manual intervention, machine lock, or mirror imaging may shift the workpiece coordinate system. Before attempting to operate the machine under the control of a program, confirm the coordinate system carefully.

If the machine is operated under the control of a program without making allowances for any shift in the workpiece coordinate system, the machine may behave unexpectedly, possibly damaging the tool, the machine itself, the workpiece, or causing injury to the operator.

8Software operator's panel and menu switches

Using the software operator's panel and menu switches, in combination with the

MDI unit, it is possible to specify operations not supported by the machine operator's panel, such as mode change, override value change, and jog feed commands.

Note, however, that if the MDI unit keys are operated inadvertently, the machine may behave unexpectedly, possibly damaging the tool, the machine itself, the workpiece, or causing injury to the user.

9RESET key

Pressing the RESET key stops the currently running program. As a result, the servo axes are stopped. However, the RESET key may fail to function for reasons such as an MDI unit problem. So, when the motors must be stopped, use the emergency stop button instead of the RESET key to ensure security.

CAUTION

1Manual intervention

If manual intervention is performed during programmed operation of the machine, the tool path may vary when the machine is restarted. Before restarting the machine after manual intervention, therefore, confirm the settings of the manual absolute switches, parameters, and absolute/incremental command mode.

2Feed hold, override, and single block

The feed hold, feedrate override, and single block functions can be disabled using custom macro system variable #3004. Be careful when operating the machine in this case.

3Dry run

Usually, a dry run is used to confirm the operation of the machine. During a dry run, the machine operates at dry run speed, which differs from the corresponding programmed feedrate. Note that the dry run speed may sometimes be higher than the programmed feed rate.

4Cutter and tool nose radius compensation in MDI mode

Pay careful attention to a tool path specified by a command in MDI mode, because cutter or tool nose radius compensation is not applied. When a command is entered from the MDI to interrupt in automatic operation in cutter or tool nose radius compensation mode, pay particular attention to the tool path when automatic operation is subsequently resumed. Refer to the descriptions of the corresponding functions for details.

s-6

B-64604EN-1/01

SAFETY PRECAUTIONS

CAUTION

5Program editing

If the machine is stopped, after which the machining program is edited (modification, insertion, or deletion), the machine may behave unexpectedly if machining is resumed under the control of that program. Basically, do not modify, insert, or delete commands from a machining program while it is in use.

WARNINGS RELATED TO DAILY MAINTENANCE

WARNING

1Memory backup battery replacement

When replacing the memory backup batteries, keep the power to the machine (CNC) turned on, and apply an emergency stop to the machine. Because this work is performed with the power on and the cabinet open, only those personnel who have received approved safety and maintenance training may perform this work.

When replacing the batteries, be careful not to touch the high-voltage circuits

(marked and fitted with an insulating cover).

Touching the uncovered high-voltage circuits presents an extremely dangerous electric shock hazard.

NOTE

The CNC uses batteries to preserve the contents of its memory, because it must retain data such as programs, offsets, and parameters even while external power is not applied.

If the battery voltage drops, a low battery voltage alarm is displayed on the machine operator's panel or screen.

When a low battery voltage alarm is displayed, replace the batteries within a week. Otherwise, the contents of the CNC's memory will be lost.

Refer to the Section "METHOD OF REPLACING BATTERY" in the Chapter, "ROUTINE MAINTENANCE" of OPERATOR’S MANUAL (Common to Lathe/Machining Center System) for details of the battery replacement procedure.

WARNING

2Absolute pulse coder battery replacement

When replacing the memory backup batteries, keep the power to the machine (CNC) turned on, and apply an emergency stop to the machine. Because this work is performed with the power on and the cabinet open, only those personnel who have received approved safety and maintenance training may perform this work.

When replacing the batteries, be careful not to touch the high-voltage circuits

(marked and fitted with an insulating cover).

Touching the uncovered high-voltage circuits presents an extremely dangerous electric shock hazard.

s-7

SAFETY PRECAUTIONS

B-64604EN-1/01

NOTE

The absolute pulse coder uses batteries to preserve its absolute position. If the battery voltage drops, a low battery voltage alarm is displayed on the machine operator's panel or screen.

When a low battery voltage alarm is displayed, replace the batteries within a week. Otherwise, the absolute position data held by the pulse coder will be lost. Refer to the FANUC SERVO MOTOR αi series Maintenance Manual for details of the battery replacement procedure.

WARNING

3Fuse replacement

Before replacing a blown fuse, however, it is necessary to locate and remove the cause of the blown fuse.

For this reason, only those personnel who have received approved safety and maintenance training may perform this work.

When replacing a fuse with the cabinet open, be careful not to touch the

high-voltage circuits (marked and fitted with an insulating cover). Touching an uncovered high-voltage circuit presents an extremely dangerous electric shock hazard.

s-8

	B-64604EN-1/01				TABLE OF CONTENTS
	TABLE OF CONTENTS
	SAFETY PRECAUTIONS...........................................................................					S-1
		DEFINITION OF WARNING, CAUTION, AND NOTE .............................................				s-1
		GENERAL WARNINGS AND CAUTIONS...............................................................				s-2
		WARNINGS AND CAUTIONS RELATED TO PROGRAMMING ............................				s-3
		WARNINGS AND CAUTIONS RELATED TO HANDLING......................................				s-5
		WARNINGS RELATED TO DAILY MAINTENANCE...............................................				s-7
	I. GENERAL
	1	GENERAL		...............................................................................................		3
		1.1	GENERAL FLOW OF OPERATION OF CNC MACHINE TOOL ...................			5
		1.2	NOTES ON READING THIS MANUAL..........................................................			6
		1.3	NOTES ON VARIOUS KINDS OF DATA ......................................................			7
	II. PROGRAMMING
	1	GENERAL .............................................................................................				11
		1.1	OFFSET ......................................................................................................			11
	2 PREPARATORY ......................................FUNCTION (G FUNCTION)					12
	3	INTERPOLATION ..............................................................FUNCTION				16
		3.1	POLAR .........................COORDINATE INTERPOLATION (G12.1, G13.1)			16
		3.2	CONSTANT ......................................................LEAD THREADING (G32)			24
		3.3	VARIABLE .........................................................LEAD THREADING (G34)			27
		3.4	CIRCULAR .........................................................THREADING (G35, G36)			28
		3.5	CONTINUOUS .......................................................................THREADING			31
		3.6	MULTIPLE .............................................................................THREADING			32
	4 FUNCTIONS .....................................TO SIMPLIFY PROGRAMMING					34
		4.1	CANNED .............................................................CYCLE (G90, G92, G94)			34
			4.1.1 ........................................Outer Diameter/Internal Diameter Cutting Cycle (G90)			35
			.........................................................................................	4.1.1.1	Straight cutting cycle	35
			............................................................................................	4.1.1.2	Taper cutting cycle	36
			4.1.2 ...........................................................................................	Threading Cycle (G92)		37
			.....................................................................................	4.1.2.1	Straight threading cycle	37
			........................................................................................	4.1.2.2	Taper threading cycle	40
			4.1.3 ..............................................................................End Face Turning Cycle (G94)			43
			..............................................................................................	4.1.3.1	Face cutting cycle	43
			............................................................................................	4.1.3.2	Taper cutting cycle	44
			4.1.4 ........................................................How to Use Canned Cycles (G90, G92, G94)			45
			4.1.5 .............................................Canned Cycle and Tool Nose Radius Compensation			47
			4.1.6 ...............................................................................Restrictions on Canned Cycles			48
		4.2	MULTIPLE ..............................REPETITIVE CANNED CYCLE (G70-G76)			51
			4.2.1 ...........................................................................Stock Removal in Turning (G71)			52
			4.2.2 .............................................................................Stock Removal in Facing (G72)			66
			4.2.3 .........................................................................................	Pattern Repeating (G73)		70
			4.2.4 ............................................................................................	Finishing Cycle (G70)		74

c-1

TABLE OF CONTENTS			B-64604EN-1/01
	4.2.5	End Face Peck Drilling Cycle (G74)......................................................................		78
	4.2.6	Outer Diameter / Internal Diameter Drilling Cycle (G75) .....................................		80
	4.2.7	Multiple Threading Cycle (G76)............................................................................		82
	4.2.8	Restrictions on Multiple Repetitive Canned Cycle (G70-G76)..............................		87
4.3	CANNED CYCLE FOR DRILLING...............................................................			90
	4.3.1	Front Drilling Cycle (G83)/Side Drilling Cycle (G87) ..........................................		93
	4.3.2	Front Tapping Cycle (G84) / Side Tapping Cycle (G88).......................................		97
	4.3.3	Front Boring Cycle (G85) / Side Boring Cycle (G89) .........................................		101
	4.3.4	Canned Cycle for Drilling Cancel (G80)..............................................................		102
	4.3.5	Addition of M Code for Clamp/Unclamp in Canned Cycle for Drilling with......		102

4.3.6Reducing of Waiting Time of Spindle Speed Arrival in the Canned Cycle for

	Drilling	.................................................................................................................	103
	4.3.7 Precautions to be Taken by Operator ...................................................................		105
4.4	RIGID TAPPING........................................................................................		106
	4.4.1 Front Face Rigid Tapping Cycle (G84) / Side Face Rigid Tapping Cycle (G88) 107
	4.4.2 Peck Rigid .............................................................Tapping Cycle (G84 or G88)		112
	4.4.3 Canned .................................................................................Cycle Cancel (G80)		116
	4.4.4 Override ............................................................................during Rigid Tapping		116
	4.4.4.1 ..........................................................................................	Extraction override	116
	4.4.4.2 ................................................................................................	Override signal	117
4.5	CANNED GRINDING .....................CYCLE (FOR GRINDING MACHINE)		119
	4.5.1 Traverse ............................................................................Grinding Cycle (G71)		121
	4.5.2 Traverse .........................................Direct Constant-Size Grinding Cycle (G72)		123
	4.5.3 Oscillation ........................................................................Grinding Cycle (G73)		125
	4.5.4 Oscillation ......................................Direct Constant-Size Grinding Cycle (G74)		127
4.6	CHAMFERING ..............................................................AND CORNER R		129
4.7	MIRROR IMAGE .............................FOR DOUBLE TURRET (G68, G69)		135
4.8	DIRECT DRAWING .................................DIMENSION PROGRAMMING		136

5 COMPENSATION FUNCTION ............................................................			142
5.1	TOOL OFFSET..........................................................................................		142
	5.1.1 Tool Geometry Offset and Tool Wear Offset.......................................................		142
	5.1.2 T Code for Tool Offset.........................................................................................		143
	5.1.3	Tool Selection.......................................................................................................	144
	5.1.4	Offset Number......................................................................................................	144
	5.1.5	Offset....................................................................................................................	144
	5.1.6	Y-Axis Offset .......................................................................................................	147
		5.1.6.1 Support of arbitrary axes for Y axis offset ......................................................	147
	5.1.7 2nd Geometry Tool Offset ...................................................................................		148
	5.1.8	4th/5th Axis Offset ...............................................................................................	150
5.2	OVERVIEW OF TOOL NOSE RADIUS COMPENSATION (G40-G42) .....		153
	5.2.1	Imaginary Tool Nose............................................................................................	153
	5.2.2 Direction of Imaginary Tool Nose .......................................................................		155
	5.2.3 Offset Number and Offset Value..........................................................................		156
	5.2.4 Workpiece Position and Move Command............................................................		157
	5.2.5 Notes on Tool Nose Radius Compensation..........................................................		162
5.3	OVERVIEW OF CUTTER COMPENSATION (G40-G42)..........................		165
5.4	DETAILS OF CUTTER OR TOOL NOSE RADIUS COMPENSATION......		171
	5.4.1	Overview ..............................................................................................................	171
	5.4.2 Tool Movement in Start-up ..................................................................................		175
	5.4.3 Tool Movement in Offset Mode...........................................................................		181
	5.4.4 Tool Movement in Offset Mode Cancel...............................................................		200
	5.4.5 Prevention of Overcutting Due to Cutter or Tool Nose Radius Compensation ...		206

c-2

B-64604EN-1/01	TABLE OF CONTENTS
	5.4.6 Interference Check ...............................................................................................	209
	5.4.6.1 Operation to be performed if an interference is judged to occur .....................	213
	5.4.6.2 Interference check alarm function ...................................................................	213
	5.4.6.3 Interference check avoidance function ............................................................	215
	5.4.7 Cutter or Tool Nose Radius Compensation for Input from MDI .........................	220
5.5	VECTOR RETENTION (G38)....................................................................	222
5.6	CORNER CIRCULAR INTERPOLATION (G39) ........................................	223
5.7	EXTENDED TOOL SELECTION ...............................................................	225
5.8	AUTOMATIC TOOL OFFSET (G36, G37).................................................	228
6 MEMORY OPERATION USING Series 10/11 FORMAT....................		231

6.1ADDRESSES AND SPECIFIED RANGE FOR Series 10/11 PROGRAM

		FORMAT ...................................................................................................			231
	6.2	SUBPROGRAM CALLING ........................................................................			231
	6.3	CANNED CYCLE.......................................................................................			232
		6.3.1	Outer Diameter/Internal Diameter Cutting Cycle (G90) ......................................		233
			6.3.1.1	Straight cutting cycle .......................................................................................	233
			6.3.1.2	Taper cutting cycle ..........................................................................................	234
		6.3.2	Threading Cycle (G92).........................................................................................		235
			6.3.2.1	Straight threading cycle ...................................................................................	235
			6.3.2.2	Taper threading cycle ......................................................................................	238
		6.3.3	End Face Turning Cycle (G94) ............................................................................		241
			6.3.3.1	Face cutting cycle ............................................................................................	241
			6.3.3.2	Taper cutting cycle ..........................................................................................	242
		6.3.4	How to Use Canned Cycles..................................................................................		244
		6.3.5	Canned Cycle and Tool Nose Radius Compensation...........................................		245
		6.3.6	Restrictions on Canned Cycles.............................................................................		246
	6.4	MULTIPLE REPETITIVE CANNED CYCLE ..............................................			249
		6.4.1	Stock Removal in Turning (G71).........................................................................		250
		6.4.2	Stock Removal in Facing (G72) ...........................................................................		260
		6.4.3	Pattern Repeating (G73).......................................................................................		264
		6.4.4	Finishing Cycle (G70)..........................................................................................		267
		6.4.5	End Face Peck Drilling Cycle (G74)....................................................................		271
		6.4.6	Outer Diameter / Internal Diameter Drilling Cycle (G75) ...................................		273
		6.4.7	Multiple Threading Cycle (G76)..........................................................................		275
		6.4.8	Restrictions on Multiple Repetitive Canned Cycle ..............................................		281
	6.5	CANNED CYCLE FOR DRILLING.............................................................			283
		6.5.1	High-speed Peck Drilling Cycle (G83.1) .............................................................		287
		6.5.2	Drilling Cycle, Spot Drilling Cycle (G81) ...........................................................		288
		6.5.3	Drilling Cycle, Counter Boring (G82) .................................................................		289
		6.5.4	Peck Drilling Cycle (G83)....................................................................................		290
		6.5.5	Tapping Cycle (G84)............................................................................................		292
		6.5.6	Tapping Cycle (G84.2).........................................................................................		293
		6.5.7	Boring Cycle (G85) ..............................................................................................		295
		6.5.8	Boring Cycle (G89) ..............................................................................................		296
		6.5.9	Canned Cycle for Drilling Cancel (G80)..............................................................		297
		6.5.10	Precautions to be Taken by Operator ...................................................................		297
7	AXIS CONTROL FUNCTIONS............................................................				298
	7.1	POLYGON TURNING (G50.2, G51.2).......................................................			298
8	MUITI-PATH CONTROL FUNCTION..................................................				303
	8.1	BALANCE CUT (G68, G69).......................................................................			303

c-3

TABLE OF CONTENTS B-64604EN-1/01

III. OPERATION
1 DATA INPUT/OUTPUT .......................................................................		307
1.1	INPUT/OUTPUT ON EACH SCREEN .......................................................	307
	1.1.1 Inputting and Outputting Y-axis Offset Data .......................................................	307
	1.1.1.1 Inputting Y-axis offset data .............................................................................	307
	1.1.1.2 Outputting Y-axis Offset Data.........................................................................	308
	1.1.2 Inputting and Outputting Tool Offset / 2nd Geometry Data ................................	309
	1.1.2.1 Inputting tool offset / 2nd geometry data.........................................................	309
	1.1.2.2 Outputting tool offset / 2nd geometry data......................................................	310
	1.1.3 Inputting and Outputting 4th/5th Axis Offset Data..............................................	311
	1.1.3.1 Inputting 4th/5th axis offset data .....................................................................	311
	1.1.3.2 Outputting 4th/5th Axis Offset Data................................................................	312
1.2	INPUT/OUTPUT ON THE ALL IO SCREEN..............................................	314
	1.2.1 Inputting and Outputting Y-axis Offset Data .......................................................	315
	1.2.2 Inputting and Outputting Tool Offset / 2nd Geometry Tool Offset .....................	316

2 SETTING AND DISPLAYING DATA...................................................										319
2.1	SCREENS DISPLAYED BY FUNCTION KEY									319
									...................................
	2.1.1 Setting and Displaying the Tool Offset Value .....................................................									319
	2.1.2 Direct Input of Tool Offset Value ........................................................................									324
	2.1.3 Direct Input of Tool Offset Value Measured B....................................................									327
	2.1.4 Counter Input of Offset value...............................................................................									329
	2.1.5 Setting the Workpiece Coordinate System Shift Value........................................									330
	2.1.6 Setting Tool Offset / 2nd Geometry Tool Offset Values......................................									334
	2.1.7 Setting the Y-Axis Offset .....................................................................................									337
	2.1.8 Setting the 4th/5th Axis Offset.............................................................................									343
	2.1.9 Chuck and Tail Stock Barriers .............................................................................									348
APPENDIX

A PARAMETERS....................................................................................		359
A.1	DESCRIPTION OF PARAMETERS...........................................................	359
A.2	DATA TYPE...............................................................................................	408
A.3	STANDARD PARAMETER SETTING TABLES.........................................	409
B LIST OF FUNCTIONS INCLUDE ADDRESS P IN THE PROGRAM
COMMAND..........................................................................................		410
B.1	LIST OF FUNCTIONS INCLUDE ADDRESS P IN THE ARGUMENT OF
	G CODE ....................................................................................................	410
B.2	LIST OF FUNCTIONS INCLUDE ADDRESS P IN THE ARGUMENT OF
	M AND S CODE ........................................................................................	414

c-4

I. GENERAL

B-64604EN-1/01

GENERAL

1.GENERAL

1 GENERAL

This manual consists of the following parts:

About this manual

I.GENERAL

Describes chapter organization, applicable models, related manuals, and notes for reading this manual.

II.PROGRAMMING

Describes each function: Format used to program functions in the NC language, characteristics, and restrictions.

III.OPERATION

Describes the manual operation and automatic operation of a machine, procedures for inputting and outputting data, and procedures for editing a program.

APPENDIX

Lists parameters.

NOTE

1This manual describes the functions that can operate in the CNC model for lathe system (path control type). For other functions not specific to the lathe system, refer to the Operator's Manual (Common to Lathe System/Machining Center

System) (B-64604EN).

2This manual does not detail the parameters not mentioned in the text. For details of those parameters, refer to the Parameter Manual (B-64610EN).

Parameters are used to set functions and operating conditions of a CNC machine tool, and frequently-used values in advance. Usually, the machine tool builder factory-sets parameters so that the user can use the machine tool easily.

3This manual describes not only basic functions but also optional functions. Look up the options incorporated into your system in the manual written by the machine tool builder.

Applicable models

This manual describes the models indicated in the table below.

In the text, the abbreviations indicated below may be used.

Model name		Abbreviation
FANUC Series 0i-TF	0i-TF	Series 0i-F	Series 0i

NOTE

1For explanatory purposes, the following descriptions may be used according to the CNC model :

- 0i-TF : Lathe system (T series)

2For the FANUC Series 0i-MODEL F, parameters need to be set to enable or disable some basic functions. For these parameters, refer to "PARAMETERS

OF 0i-F BASIC FUNCTIONS" in the PARAMETER MANUAL (B-64610EN).

-3 -

1.GENERAL

GENERAL

B-64604EN-1/01

Special symbols

This manual uses the following symbols:

-IP

Indicates a combination of axes such as X_ Y_ Z_

In the underlined position following each address, a numeric value such as a coordinate value is placed (used in PROGRAMMING.).

-;

Indicates the end of a block. It actually corresponds to the ISO code LF or EIA code CR.

Related manuals of Series 0i- MODEL F

The following table lists the manuals related to Series 0i-F. This manual is indicated by an asterisk(*).

Table 1 (a) Related manuals

Manual name	Specification number
DESCRIPTIONS	B-64602EN
CONNECTION MANUAL (HARDWARE)	B-64603EN
CONNECTION MANUAL (FUNCTION)	B-64603EN-1
OPERATOR’S MANUAL (Common to Lathe System/Machining Center System)	B-64604EN
OPERATOR’S MANUAL (For Lathe System)	B-64604EN-1	*
OPERATOR’S MANUAL (For Machining Center System)	B-64604EN-2
MAINTENANCE MANUAL	B-64605EN
PARAMETER MANUAL	B-64610EN
Programming
Macro Executor PROGRAMMING MANUAL	B-63943EN-2
Macro Compiler PROGRAMMING MANUAL	B-66263EN
C Language Executor PROGRAMMING MANUAL	B-63943EN-3
PMC
PMC PROGRAMMING MANUAL	B-64513EN
Network
PROFIBUS-DP Board CONNECTION MANUAL	B-63993EN
Fast Ethernet / Fast Data Server OPERATOR’S MANUAL	B-64014EN
DeviceNet Board CONNECTION MANUAL	B-64043EN
CC-Link Board CONNECTION MANUAL	B-64463EN
Operation guidance function
MANUAL GUIDE i (Common to Lathe System/Machining Center System)	B-63874EN
OPERATOR’S MANUAL
MANUAL GUIDE i (For Machining Center System) OPERATOR’S MANUAL	B-63874EN-2
MANUAL GUIDE i (Set-up Guidance Functions) OPERATOR’S MANUAL	B-63874EN-1
MANUAL GUIDE 0i OPERATOR’S MANUAL	B-64434EN
TURN MATE i OPERATOR’S MANUAL	B-64254EN
Dual Check Safety
Dual Check Safety CONNECTION MANUAL	B-64483EN-2

Related manuals of SERVO MOTOR αi/βi series

The following table lists the manuals related to SERVO MOTOR αi/βi series

Table 1 (b) Related manuals

Manual name	Specification number
FANUC AC SERVO MOTOR αi series DESCRIPTIONS	B-65262EN
FANUC AC SPINDLE MOTOR αi series DESCRIPTIONS	B-65272EN
FANUC AC SERVO MOTOR βi series DESCRIPTIONS	B-65302EN
FANUC AC SPINDLE MOTOR βi series DESCRIPTIONS	B-65312EN

- 4 -

B-64604EN-1/01		GENERAL	1.GENERAL
	Manual name		Specification number
	FANUC SERVO AMPLIFIER αi series DESCRIPTIONS		B-65282EN
	FANUC SERVO AMPLIFIER βi series DESCRIPTIONS		B-65322EN
	FANUC SERVO MOTOR αis series
	FANUC SERVO MOTOR αi series
	FANUC AC SPINDLE MOTOR αi series		B-65285EN
	FANUC SERVO AMPLIFIER αi series
	MAINTENANCE MANUAL
	FANUC SERVO MOTOR βis series
	FANUC AC SPINDLE MOTOR βi series		B-65325EN
	FANUC SERVO AMPLIFIER βi series
	MAINTENANCE MANUAL
	FANUC AC SERVO MOTOR αi series
	FANUC AC SERVO MOTOR βi series
	FANUC LINEAR MOTOR LiS series		B-65270EN
	FANUC SYNCHRONOUS BUILT-IN SERVO MOTOR DiS series
	PARAMETER MANUAL
	FANUC AC SPINDLE MOTOR αi/βi series,
	BUILT-IN SPINDLE MOTOR Bi series		B-65280EN
	PARAMETER MANUAL

The above servo motors and the corresponding spindles can be connected to the CNC covered in this manual. In the αi SV, αi SP, αi PS, and βi SV series, however, they can be connected only to 30 i-B-compatible versions. In the βi SVSP series, they cannot be connected.

This manual mainly assumes that the FANUC SERVO MOTOR αi series of servo motor is used. For servo motor and spindle information, refer to the manuals for the servo motor and spindle that are actually connected.

1.1 GENERAL FLOW OF OPERATION OF CNC MACHINE TOOL

When machining the part using the CNC machine tool, first prepare the program, then operate the CNC machine by using the program.

(1)First, prepare the program from a part drawing to operate the CNC machine tool. How to prepare the program is described in the Part II, "PROGRAMMING".

(2)The program is to be read into the CNC system. Then, mount the workpieces and tools on the machine, and operate the tools according to the programming. Finally, execute the machining actually.

How to operate the CNC system is described in the Part III, "OPERATION".

Part	Part
drawing	program
		CNC	Machine Tool
PART II, "PROGRAMMING"		PART III, "OPERATION"

Before the actual programming, make the machining plan for how to machine the part. Machining plan)

1.Determination of workpieces machining range

2.Method of mounting workpieces on the machine tool

3.Machining sequence in every cutting process

4.Cutting tools and cutting conditions

- 5 -

1.GENERAL

GENERAL

B-64604EN-1/01

Decide the cutting method in every cutting process.

Cutting process	1		2	3
Cutting procedure	End face cutting		Outer diameter cutting	Grooving
1. Cutting method :
Rough
Semi
Finish
2. Cutting tools
3. Cutting conditions :
Feedrate
Cutting depth
4. Tool path
		Outer
	Grooving	diameter	End face cutting
		cutting

Workpiece

Prepare the program of the tool path and cutting condition according to the workpiece figure, for each cutting.

1.2 NOTES ON READING THIS MANUAL

CAUTION

1The function of an CNC machine tool system depends not only on the CNC, but on the combination of the machine tool, its magnetic cabinet, the servo system, the CNC, the operator's panels, etc. It is too difficult to describe the function, programming, and operation relating to all combinations. This manual generally describes these from the stand-point of the CNC. So, for details on a particular

CNC machine tool, refer to the manual issued by the machine tool builder, which should take precedence over this manual.

2In the header field of each page of this manual, a chapter title is indicated so that the reader can reference necessary information easily.

By finding a desired title first, the reader can reference necessary parts only.

3This manual describes as many reasonable variations in equipment usage as possible. It cannot address every combination of features, options and commands that should not be attempted.

If a particular combination of operations is not described, it should not be attempted.

-6 -

B-64604EN-1/01

GENERAL

1.GENERAL

1.3 NOTES ON VARIOUS KINDS OF DATA

CAUTION

1Machining programs, parameters, offset data, etc. are stored in the CNC unit internal non-volatile memory. In general, these contents are not lost by the switching ON/OFF of the power. However, it is possible that a state can occur where precious data stored in the non-volatile memory has to be deleted, because of deletions from a maloperation, or by a failure restoration. In order to restore rapidly when this kind of mishap occurs, it is recommended that you create a copy of the various kinds of data beforehand.

2The number of times to write machining programs to the non-volatile memory is limited.

You must use "High-speed program management" when registration and the deletion of the machining programs are frequently repeated in such case that the machining programs are automatically downloaded from a personal computer at each machining.

In "High-speed program management", the program is not saved to the non-volatile memory at registration, modification, or deletion of programs.

- 7 -

II. PROGRAMMING

B-64604EN-1/01

PROGRAMMING

1.GENERAL

1 GENERAL

Chapter 1, "GENERAL", consists of the following sections:

1.1 OFFSET ..............................................................................................................................................

11

1.1 OFFSET

Explanation

-Tool offset

Usually, several tools are used for machining one workpiece. The tools have different tool length. It is very troublesome to change the program in accordance with the tools.

Therefore, the length of each tool used should be measured in advance. By setting the difference between the length of the standard tool and the length of each tool in the CNC (see Chapter, “Setting and Displaying Data” in the OPERATOR’S MANUAL (Common to Lathe System/Machining Center System)), machining can be performed without altering the program even when the tool is changed. This function is called tool offset.

Standard	Rough	Finishing	Grooving	Threading
tool	cutting	tool	tool	tool
	tool
Workpiece

Fig. 1.1 (a) Tool offset

- 11 -

2. PREPARATORY FUNCTION

(G FUNCTION) PROGRAMMING B-64604EN-1/01

2 PREPARATORY FUNCTION (G FUNCTION)

A number following address G determines the meaning of the command for the concerned block. G codes are divided into the following two types.

	Type			Meaning
One-shot G code			The G code is effective only in the block in which it is specified.
Modal G code			The G code is effective until another G code of the same group is specified.
(Example)
G01 and G00 are modal G codes in group 01.
G01	X_ ;
	Z_ ;	G01 is effective in this range.
	X_ ;
G00	Z_ ;	G00 is effective in this range.
	X_ ;
G01	X_ ;
	:

There are three G code systems in the lathe system : A,B, and C (Table 2 (a)). Select a G code system using bits 6 (GSB) and 7 (GSC) parameter No. 3401. Generally, OPERATOR’S MANUAL describes the use of G code system A, except when the described item can use only G code system B or C. In such cases, the use of G code system B or C is described.

Explanation

1.When the clear state (bit 6 (CLR) of parameter No. 3402) is set at power-up or reset, the modal G codes are placed in the states described below.

(1)The modal G codes are placed in the states marked with as indicated in Table.

(2)G20 and G21 remain unchanged when the clear state is set at power-up or reset.

(3)Which status G22 or G23 at power on is set by bit 7 (G23) of parameter No. 3402. However, G22 and G23 remain unchanged when the clear state is set at reset.

(4)The user can select G00 or G01 by setting bit 0 (G01) of parameter No. 3402.

(5)The user can select G90 or G91 by setting bit 3 (G91) of parameter No. 3402.

When G code system B or C is used in the lathe system, setting bit 3 (G91) of parameter No. 3402 determines which code, either G90 or G91, is effective.

2.G codes other than G10 and G11 are one-shot G codes.

3.When a G code not listed in the G code list is specified, or a G code that has no corresponding option is specified, alarm PS0010, “IMPROPER G-CODE” occurs.

4.Multiple G codes can be specified in the same block if each G code belongs to a different group. If multiple G codes that belong to the same group are specified in the same block, only the last G code specified is valid.

5.If a G code belonging to group 01 is specified in a for drilling, the canned cycle for drilling is cancelled. This means that the same state set by specifying G80 is set. Note that the G codes in group 01 are not affected by a G code specifying a canned cycle.

6.When G code system A is used, absolute or incremental programming is specified not by a G code (G90/G91) but by an address word (X/U, Z/W, C/H, Y/V). Only the initial level is provided at the return point of the canned cycle for drilling..

7.G codes are indicated by group.

-12 -

							2.PREPARATORY FUNCTION
B-64604EN-1/01						PROGRAMMING		(G FUNCTION)
						Table 2 (a) G code list
		G code system				Group	Function
	A		B		C
	G00		G00		G00		Positioning (Rapid traverse)
	G01		G01		G01	01	Linear interpolation (Cutting feed)
	G02		G02		G02		Circular interpolation CW or helical interpolation CW
	G03		G03		G03		Circular interpolation CCW or helical interpolation CCW
	G04		G04		G04		Dwell
	G04.1		G04.1		G04.1		G code preventing buffering
	G05.1		G05.1		G05.1		AI contour control
	G05.4		G05.4		G05.4		HRV3 on/off
	G07.1		G07.1		G07.1		Cylindrical interpolation
	(G107)		(G107)		(G107)
						00
	G08		G08		G08		AI contour control (advanced preview control compatible
							command)
	G09		G09		G09		Exact stop
	G10		G10		G10		Programmable data input
	G10.6		G10.6		G10.6		Tool retract and recover
	G11		G11		G11		Programmable data input mode cancel
	G12.1		G12.1		G12.1		Polar coordinate interpolation mode
	(G112)		(G112)		(G112)
						21
	G13.1		G13.1		G13.1		Polar coordinate interpolation cancel mode
	(G113)		(G113)		(G113)
	G17		G17		G17		XpYp plane selection
	G18		G18		G18	16	ZpXp plane selection
	G19		G19		G19		YpZp plane selection
	G20		G20		G70	06	Input in inch
	G21		G21		G71		Input in mm
	G22		G22		G22	09	Stored stroke check function on
	G23		G23		G23		Stored stroke check function off
	G25		G25		G25	08	Spindle speed fluctuation detection off
	G26		G26		G26		Spindle speed fluctuation detection on
	G27		G27		G27		Reference position return check
	G28		G28		G28		Return to reference position
	G28.2		G28.2		G28.2		In-position check disable reference position return
	G29		G29		G29	00	Movement from reference position
	G30		G30		G30		2nd, 3rd and 4th reference position return
	G30.2		G30.2		G30.2		In-position check disable 2nd, 3rd, or 4th reference position
							return
	G31		G31		G31		Skip function
	G32		G33		G33		Threading
	G34		G34		G34		Variable lead threading
	G35		G35		G35		Circular threading CW
							Circular threading CCW (When bit 3 (G36) of parameter No.
	G36		G36		G36		3405 is set to 1) or Automatic tool offset (X axis) (When bit 3
							(G36) of parameter No. 3405 is set to 0)
	G37		G37		G37	01	Automatic tool offset (Z axis) (When bit 3 (G36) of parameter
							No. 3405 is set to 0)
	G37.1		G37.1		G37.1		Automatic tool offset (X axis) (When bit 3 (G36) of parameter
							No. 3405 is set to 1)
	G37.2		G37.2		G37.2		Automatic tool offset (Z axis) (When bit 3 (G36) of parameter
							No. 3405 is set to 1)
	G38		G38		G38		Tool radius/tool nose radius compensation: with vector held
	G39		G39		G39		Tool radius/tool nose radius compensation: corner rounding
							interpolation

- 13 -

2. PREPARATORY FUNCTION

	(G FUNCTION)					PROGRAMMING		B-64604EN-1/01
						Table 2 (a) G code list
		G code system				Group	Function
	A		B		C
	G40		G40		G40		Tool radius/tool nose radius compensation : cancel
	G41		G41		G41		Tool radius/tool nose radius compensation : left
	G42		G42		G42	07	Tool radius/tool nose radius compensation : right
	G43.7		G43.7		G43.7		Tool offset
	(G44.7)		(G44.7)		(G44.7)		(Bit 3 (TCT) of parameter No. 5040 must be "1".)
	G49		G49		G49		Tool length compensation cancel
	(G49.1)		(G49.1)		(G49.1)		(Bit 3 (TCT) of parameter No. 5040 must be "1".)
	G50		G92		G92	00	Coordinate system setting or max spindle speed clamp
	G50.3		G92.1		G92.1		Workpiece coordinate system preset
	G50.1		G50.1		G50.1	22	Programmable mirror image cancel
	G51.1		G51.1		G51.1		Programmable mirror image
	G50.2		G50.2		G50.2		Polygon turning cancel
	(G250)		(G250)		(G250)
						20
	G51.2		G51.2		G51.2		Polygon turning
	(G251)		(G251)		(G251)
	G50.4		G50.4		G50.4		Cancel synchronous control
	G50.5		G50.5		G50.5		Cancel composite control
	G50.6		G50.6		G50.6		Cancel superimposed control
	G51.4		G51.4		G51.4	00	Start synchronous control
	G51.5		G51.5		G51.5		Start composite control
	G51.6		G51.6		G51.6		Start superimposed control
	G52		G52		G52		Local coordinate system setting
	G53		G53		G53		Machine coordinate system setting
	G54		G54		G54		Workpiece coordinate system 1 selection
	(G54.1)		(G54.1)		(G54.1)
	G55		G55		G55		Workpiece coordinate system 2 selection
	G56		G56		G56	14	Workpiece coordinate system 3 selection
	G57		G57		G57		Workpiece coordinate system 4 selection
	G58		G58		G58		Workpiece coordinate system 5 selection
	G59		G59		G59		Workpiece coordinate system 6 selection
	G61		G61		G61		Exact stop mode
	G62		G62		G62	15	Automatic corner override mode
	G63		G63		G63		Tapping mode
	G64		G64		G64		Cutting mode
	G65		G65		G65	00	Macro call
	G66		G66		G66		Macro modal call A
	G66.1		G66.1		G66.1	12	Macro modal call B
	G67		G67		G67		Macro modal call A/B cancel
	G68		G68		G68	04	Mirror image on for double turret or balance cutting mode
	G68.1		G68.1		G68.1	17	Coordinate system rotation start or 3-dimensional coordinate
							system conversion mode on
	G69		G69		G69	04	Mirror image off for double turret or balance cutting mode
							cancel
	G69.1		G69.1		G69.1	17	Coordinate system rotation cancel or 3-dimensional
							coordinate system conversion mode off

- 14 -

							2.PREPARATORY FUNCTION
B-64604EN-1/01						PROGRAMMING		(G FUNCTION)
						Table 2 (a) G code list
		G code system				Group	Function
	A		B		C
	G70		G70		G72		Finishing cycle
	G71		G71		G73		Stock removal in turning
	G72		G72		G74	00	Stock removal in facing
	G73		G73		G75		Pattern repeating cycle
	G74		G74		G76		End face peck drilling cycle
	G75		G75		G77		Outer diameter/internal diameter drilling cycle
	G76		G76		G78		Multiple-thread cutting cycle
	G71		G71		G72		Traverse grinding cycle
	G72		G72		G73	01	Traverse direct sizing/grinding cycle
	G73		G73		G74		Oscillation grinding cycle
	G74		G74		G75		Oscillation direct sizing/grinding cycle
	G80		G80		G80	10	Canned cycle cancel for drilling
	G81.1		G81.1		G81.1	00	High precision oscillation function
	G81		G81		G81		Spot drilling (FS10/11-T format)
	G82		G82		G82		Counter boring (FS10/11-T format)
	G83		G83		G83		Cycle for face drilling
	G83.1		G83.1		G83.1		High-speed peck drilling cycle (FS10/11-T format)
	G83.5		G83.5		G83.5		High-speed peck drilling cycle
	G83.6		G83.6		G83.6		Peck drilling cycle
	G84		G84		G84	10	Cycle for face tapping
	G84.2		G84.2		G84.2		Rigid tapping cycle (FS10/11-T format)
	G85		G85		G85		Cycle for face boring
	G87		G87		G87		Cycle for side drilling
	G87.5		G87.5		G87.5		High-speed peck drilling cycle
	G87.6		G87.6		G87.6		Peck drilling cycle
	G88		G88		G88		Cycle for side tapping
	G89		G89		G89		Cycle for side boring
	G90		G77		G20		Outer diameter/internal diameter cutting cycle
	G92		G78		G21	01	Threading cycle
	G94		G79		G24		End face turning cycle
	G91.1		G91.1		G91.1	00	Maximum specified incremental amount check
	G96		G96		G96	02	Constant surface speed control
	G97		G97		G97		Constant surface speed control cancel
	G96.1		G96.1		G96.1		Spindle indexing execution (waiting for completion)
	G96.2		G96.2		G96.2	00	Spindle indexing execution (not waiting for completion)
	G96.3		G96.3		G96.3		Spindle indexing completion check
	G96.4		G96.4		G96.4		SV speed control mode ON
	G98		G94		G94	05	Feed per minute
	G99		G95		G95		Feed per revolution
	-		G90		G90	03	Absolute programming
	-		G91		G91		Incremental programming
	-		G98		G98	11	Canned cycle : return to initial level
	-		G99		G99		Canned cycle : return to R point level

- 15 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64604EN-1/01

3 INTERPOLATION FUNCTION

Chapter 3, "INTERPOLATION FUNCTION", consists of the following sections:

3.1	POLAR COORDINATE INTERPOLATION (G12.1, G13.1)...........................................................	16
3.2	CONSTANT LEAD THREADING (G32) .........................................................................................	24
3.3	VARIABLE LEAD THREADING (G34) ..........................................................................................	27
3.4	CIRCULAR THREADING (G35, G36).............................................................................................	28
3.5	CONTINUOUS THREADING...........................................................................................................	31
3.6	MULTIPLE THREADING.................................................................................................................	32

3.1 POLAR COORDINATE INTERPOLATION (G12.1, G13.1)

Overview

Polar coordinate interpolation is a function that exercises contour control in converting a command programmed in a Cartesian coordinate system to the movement of a linear axis (movement of a tool) and the movement of a rotary axis (rotation of a workpiece). This function is useful for grinding a cam shaft.

NOTE

When bit 5 (NPI) of parameter No.8137 is 0, this function can be used.

Format

G12.1; Starts polar coordinate interpolation mode (enables polar coordinate interpolation).

Specify linear or circular interpolation using coordinates in a Cartesian coordinate system consisting of a linear axis and rotary axis (hypothetical axis).

G13.1; Polar coordinate interpolation mode is cancelled (for not performing polar coordinate interpolation).

Specify G12.1 and G13.1 in Separate Blocks.

Explanation

-Polar coordinate interpolation mode (G12.1)

The axes of polar coordinate interpolation (linear axis and rotary axis) should be specified in advance, with corresponding parameters. Specifying G12.1 places the system in the polar coordinate interpolation mode, and selects a plane (called the polar coordinate interpolation plane) formed by one linear axis and a hypothetical axis intersecting the linear axis at right angles. The linear axis is called the first axis of the plane, and the hypothetical axis is called the second axis of the plane. Polar coordinate interpolation is performed in this plane.

In the polar coordinate interpolation mode, both linear interpolation and circular interpolation can be specified by absolute or incremental programming.

Tool radius compensation can also be performed. The polar coordinate interpolation is performed for a path obtained after tool radius compensation.

The tangential velocity in the polar coordinate interpolation plane (Cartesian coordinate system) is specified as the feedrate, using F.

- Polar coordinate interpolation cancel mode (G13.1)

Specifying G13.1 cancels the polar coordinate interpolation mode.

- 16 -