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

1 Never 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.

2 Before 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.

3 Ensure 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.

4 When 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.

5 The 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

1 Immediately 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.

2 The 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.

3 Some 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

4 The 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

1 Programs, 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.

2 The 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

Coordinate 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.

Positioning 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.

Function 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

Inch/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.

Constant 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.

Stroke 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.

Interference 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.

Same 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

Absolute/incremental mode

If a program created with absolute values is run in incremental mode, or vice

versa, the machine may behave unexpectedly.

Plane 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.

Torque 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.

Programmable mirror image

Note that programmed operations vary considerably when a programmable

mirror image is enabled.

s-4

B-64604EN-1/01 SAFETY PRECAUTIONS

CAUTION

Compensation 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

Manual 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.

Manual 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.

Manual 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.

Manual 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.

Disabled 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.

Origin/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

Workpiece 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.

Software 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.

RESET 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

Manual 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.

Feed 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.

Dry 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.

Cutter 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

Program 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

Memory backup battery replacement

When replacing the memory backup batteries, keep the power to the machine

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

Absolute 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

series Maintenance Manual for details

of the battery replacement procedure.

WARNING

Fuse 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

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

4.3.6 Reducing 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

6.1 ADDRESSES 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

1 This 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).

2 This 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.

3 This 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

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

the CNC model :

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

2 For 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) OPERATOR’S MANUAL MANUAL GUIDE i (For Machining Center System) OPERATOR’S MANUAL MANUAL GUIDE i (Set-up Guidance Functions) OPERATOR’S MANUAL MANUAL GUIDE 0i OPERATOR’S MANUAL TURN MATE i OPERATOR’S MANUAL

Dual Check Safety

Dual Check Safety CONNECTION MANUAL B-64483EN-2

B-63874EN

B-63874EN-2 B-63874EN-1 B-64434EN B-64254EN

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 FANUC AC SPINDLE MOTOR αi series DESCRIPTIONS FANUC AC SERVO MOTOR βi series DESCRIPTIONS FANUC AC SPINDLE MOTOR βi series DESCRIPTIONS

- 4 -

B-65262EN B-65272EN B-65302EN B-65312EN

B-64604EN-1/01 GENERAL 1.GENERAL

Manual name Specification number

FANUC SERVO AMPLIFIER αi series DESCRIPTIONS FANUC SERVO AMPLIFIER βi series DESCRIPTIONS FANUC SERVO MOTOR αis series FANUC SERVO MOTOR αi series FANUC AC SPINDLE MOTOR αi series FANUC SERVO AMPLIFIER αi series MAINTENANCE MANUAL FANUC SERVO MOTOR βis series FANUC AC SPINDLE MOTOR βi series FANUC SERVO AMPLIFIER βi series MAINTENANCE MANUAL FANUC AC SERVO MOTOR αi series FANUC AC SERVO MOTOR βi series FANUC LINEAR MOTOR LiS series FANUC SYNCHRONOUS BUILT-IN SERVO MOTOR DiS series PARAMETER MANUAL FANUC AC SPINDLE MOTOR αi/βi series, BUILT-IN SPINDLE MOTOR Bi series PARAMETER MANUAL

B-65282EN B-65322EN

B-65285EN

B-65325EN

B-65270EN

B-65280EN

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 drawing

PART II, "PROGRAMMING"

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

Part program

CNC Machine Tool

PART III, "OPERATION"

- 5 -

1.GENERAL GENERAL B-64604EN-1/01

Decide the cutting method in every cutting process.

1 2 3 Cutting process

Cutting procedure

1. Cutting method : Rough Semi Finish

2. Cutting tools

3. Cutting conditions : Feedrate Cutting depth

4. Tool path

End face cutting Outer diameter cutting Grooving

Outer

Grooving

diameter cutting

Workpiece

End face cutting

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

1 The 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.

2 In 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.

3 This 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

1 Machining 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.

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

- 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 tool

Rough cutting tool

Finishing tool

Grooving tool

Threading 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 (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.

as indicated in Table.

- 12 -

2.PREPARATORY FUNCTION

B-64604EN-1/01 PROGRAMMING

Table 2 (a) G code list

G code system

A B C

G00 G00 G00 Positioning (Rapid traverse) G01 G01 G01 Linear interpolation (Cutting feed) G02 G02 G02 Circular interpolation CW or helical interpolation CW G03 G03 G03

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

(G107)

G08 G08 G08

G09 G09 G09 Exact stop

G10 G10 G10 Programmable data input G10.6 G10.6 G10.6 Tool retract and recover

G11 G11 G11 G12.1

(G112)

G13.1

(G113)

G17 G17 G17 XpYp plane selection

G18 G18 G18 ZpXp plane selection

G19 G19 G19

G20 G20 G70 Input in inch

G21 G21 G71

G22 G22 G22 Stored stroke check function on

G23 G23 G23

G25 G25 G25 Spindle speed fluctuation detection off

G26 G26 G26

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 Movement from reference position

G30 G30 G30 2nd, 3rd and 4th reference position return G30.2 G30.2 G30.2

G31 G31 G31

G32 G33 G33 Threading

G34 G34 G34 Variable lead threading

G35 G35 G35 Circular threading CW

G36 G36 G36

G37 G37 G37

G37.1 G37.1 G37.1

G37.2 G37.2 G37.2

G38 G38 G38 Tool radius/tool nose radius compensation: with vector held

G39 G39 G39

G07.1

(G107)

G12.1

(G112)

G13.1

(G113)

G07.1

(G107)

G12.1

(G112)

G13.1

(G113)

Group Function

Circular interpolation CCW or helical interpolation CCW

Cylindrical interpolation

AI contour control (advanced preview control compatible command)

Programmable data input mode cancel Polar coordinate interpolation mode

Polar coordinate interpolation cancel mode

YpZp plane selection

Input in mm

Stored stroke check function off

Spindle speed fluctuation detection on

In-position check disable 2nd, 3rd, or 4th reference position return Skip function

Circular threading CCW (When bit 3 (G36) of parameter No. 3405 is set to 1) or Automatic tool offset (X axis) (When bit 3 (G36) of parameter No. 3405 is set to 0) Automatic tool offset (Z axis) (When bit 3 (G36) of parameter No. 3405 is set to 0) Automatic tool offset (X axis) (When bit 3 (G36) of parameter No. 3405 is set to 1) Automatic tool offset (Z axis) (When bit 3 (G36) of parameter No. 3405 is set to 1)

Tool radius/tool nose radius compensation: corner rounding interpolation

(G FUNCTION)

- 13 -

2. PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING B-64604EN-1/01

Table 2 (a) G code list

G code system

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 Tool radius/tool nose radius compensation : right

G43.7

(G44.7)

G49

(G49.1)

G50 G92 G92 Coordinate system setting or max spindle speed clamp G50.3 G92.1 G92.1 G50.1 G50.1 G50.1 Programmable mirror image cancel G51.1 G51.1 G51.1 G50.2

(G250)

G51.2

(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 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

G54

(G54.1)

G55 G55 G55 Workpiece coordinate system 2 selection

G56 G56 G56 Workpiece coordinate system 3 selection

G57 G57 G57 Workpiece coordinate system 4 selection

G58 G58 G58 Workpiece coordinate system 5 selection

G59 G59 G59

G61 G61 G61 Exact stop mode

G62 G62 G62 Automatic corner override mode

G63 G63 G63 Tapping mode

G64 G64 G64

G65 G65 G65 00 Macro call

G66 G66 G66 Macro modal call A G66.1 G66.1 G66.1 Macro modal call B

G67 G67 G67

G68 G68 G68 04 Mirror image on for double turret or balance cutting mode G68.1 G68.1 G68.1 17

G69 G69 G69

G69.1 G69.1 G69.1 17

G43.7

(G44.7)

G49

(G49.1)

G50.2

(G250)

G51.2

(G251)

G54

(G54.1)

G43.7

(G44.7)

G49

(G49.1)

G50.2

(G250)

G51.2

(G251)

G54

(G54.1)

Group Function

04 Mirror image off for double turret or balance cutting mode

Tool offset (Bit 3 (TCT) of parameter No. 5040 must be "1".) Tool length compensation cancel (Bit 3 (TCT) of parameter No. 5040 must be "1".)

Workpiece coordinate system preset

Programmable mirror image Polygon turning cancel

Polygon turning

Machine coordinate system setting Workpiece coordinate system 1 selection

Workpiece coordinate system 6 selection

Cutting mode

Macro modal call A/B cancel

Coordinate system rotation start or 3-dimensional coordinate system conversion mode on

cancel Coordinate system rotation cancel or 3-dimensional coordinate system conversion mode off

- 14 -

2.PREPARATORY FUNCTION

B-64604EN-1/01 PROGRAMMING

Table 2 (a) G code list

G code system

A B C

G70 G70 G72 Finishing cycle

G71 G71 G73 Stock removal in turning

G72 G72 G74 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

G71 G71 G72 Traverse grinding cycle

G72 G72 G73 Traverse direct sizing/grinding cycle

G73 G73 G74 Oscillation grinding cycle

G74 G74 G75

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 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

G90 G77 G20 Outer diameter/internal diameter cutting cycle

G92 G78 G21 Threading cycle

G94 G79 G24 G91.1 G91.1 G91.1 00 Maximum specified incremental amount check

G96 G96 G96 Constant surface speed control

G97 G97 G97 G96.1 G96.1 G96.1 Spindle indexing execution (waiting for completion) G96.2 G96.2 G96.2 Spindle indexing execution (not waiting for completion) G96.3 G96.3 G96.3 Spindle indexing completion check G96.4 G96.4 G96.4

G98 G94 G94 Feed per minute

G99 G95 G95

- G90 G90 Absolute programming

- G91 G91

- G98 G98 Canned cycle : return to initial level

- G99 G99

Group Function

Multiple-thread cutting cycle

Oscillation direct sizing/grinding cycle

Cycle for side boring

End face turning cycle

Constant surface speed control cancel

SV speed control mode ON

Feed per revolution

Incremental programming

Canned cycle : return to R point level

(G FUNCTION)

- 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 -

+ 402 hidden pages