fanuc 0i- F Operators Manual

Download

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 -

B-64604EN-1/01 PROGRAMMING 3.INTERPOLATION FUNCTION

- Polar coordinate interpolation plane

G12.1 starts the polar coordinate interpolation mode and selects a polar coordinate interpolation plane (Fig. 3.1 (a)). Polar coordinate interpolation is performed on this plane.

Rotary axis (hypothetical axis)

(unit: mm or inch)

Linear axis (unit: mm or inch)

Origin of the local coordinate system (G52 command) (Or origin of the workpiece coordinate system)

Fig. 3.1 (a) Polar coordinate interpolation plane

When the power is turned on or the system is reset, polar coordinate interpolation is canceled (G13.1). The linear and rotation axes for polar coordinate interpolation must be set in parameters Nos. 5460 and 5461 beforehand.

CAUTION

The plane used before G12.1 is specified (plane selected by G17, G18, or G19)

is canceled. It is restored when G13.1 (canceling polar coordinate interpolation) is specified.

When the system is reset, polar coordinate interpolation is canceled and the

plane specified by G17, G18, or G19 is used.

- Distance moved and feedrate for polar coordinate interpolation

• The unit for coordinates on the hypothetical axis is the same as the unit for the linear axis (mm/inch). In the polar coordinate interpolation mode, program commands are specified with Cartesian

coordinates on the polar coordinate interpolation plane. The axis address for the rotary axis is used as the axis address for the second axis (hypothetical axis) in the plane. Whether a diameter or radius is specified for the first axis in the plane is the same as for the rotary axis regardless of the specification for the first axis in the plane.

The hypothetical axis is at coordinate 0 immediately after G12.1 is specified. Polar interpolation is

started assuming the rotation angle of 0 for the position of the tool when G12.1 is specified. Example) When a value on the X-axis (linear axis) is input in millimeters G12.1;

G01 X10.0 F1000. ; ......A 10.0-mm movement is made on the Cartesian coordinate system.

C20.0 ;...........................A 20.0-mm movement is made on the Cartesian coordinate system.

G13.1;

When a value on the X-axis (linear axis) is input in inches G12.1;

G01 X10.0 F1000. ; .... A 10.0-inch movement is made on the Cartesian coordinate system.

C20.0 ;...........................A 20.0-inch movement is made on the Cartesian coordinate system.

G13.1;

• The unit for the feedrate is mm/min or inch/min.

- 17 -

3.INTERPOLATION FUNCTION PROGRAMMING B-64604EN-1/01

Specify the feedrate as a speed (relative speed between the workpiece and tool) tangential to the

polar coordinate interpolation plane (Cartesian coordinate system) using F.

- G codes which can be specified in the polar coordinate interpolation mode

G01.......................Linear interpolation

G02, G03..............Circular interpolation

G04.......................Dwell, Exact stop

G40, G41, G42 .....Tool radius compensation (Polar coordinate interpolation is applied to the path

after tool radius compensation.)

G65, G66, G67 .....Custom macro command

G90, G91..............Absolute programming, incremental programming (For G code system B or C)

G94, G95..............Feed per minute, feed per revolution

- Circular interpolation in the polar coordinate plane

The addresses for specifying the radius of an arc for circular interpolation (G02 or G03) in the polar coordinate interpolation plane depend on the first axis in the plane (linear axis).

• I and J in the Xp-Yp plane when the linear axis is the X-axis or an axis parallel to the X-axis.

• J and K in the Yp-Zp plane when the linear axis is the Y-axis or an axis parallel to the Y-axis.

• K and I in the Zp-Xp plane when the linear axis is the Z-axis or an axis parallel to the Z-axis.

The radius of an arc can be specified also with an R command.

NOTE

The parallel axes U, V, and W can be used in the G code system B or C.

- Movement along axes not in the polar coordinate interpolation plane in the polar coordinate interpolation mode

The tool moves along such axes normally, independent of polar coordinate interpolation.

- Current position display in the polar coordinate interpolation mode

Actual coordinates are displayed. However, the remaining distance to move in a block is displayed based on the coordinates in the polar coordinate interpolation plane (Cartesian coordinates).

- Coordinate system for the polar coordinate interpolation

Basically, before G12.1 is specified, a local coordinate system (or workpiece coordinate system) where the center of the rotary axis is the origin of the coordinate system must be set. In the G12.1 mode, the coordinate system must not be changed (G50, G52, G53, relative coordinate reset, G54 through G59, etc.).

- Compensation in the direction of the hypothetical axis in polar coordinate interpolation

If the first axis of the plane has an error from the center of the rotary axis in the hypothetical axis direction, in other words, if the rotary axis center is not on the X-axis, the hypothetical axis direction compensation function in the polar coordinate interpolation mode is used. With the function, the error is considered in polar coordinate interpolation. The amount of error is specified in parameter No. 5464.

- 18 -

B-64604EN-1/01 PROGRAMMING 3.INTERPOLATION FUNCTION

Hypothetical axis (C-axis)

Rotary axis

(X, C)

Error in the direction of hypothetical axis (P)

Center of rotary axis

(X, C) : Point in the X-C plane (The center of the rotary axis is considered to be the origin of

the X-C plane.) X : X coordinate in the X-C plane C : Hypothetical axis coordinate in the X-C plane P : Error in the direction of the hypothetical axis (specified in parameter No. 5464)

X-axis

- Shifting the coordinate system in polar coordinate interpolation

In the polar coordinate interpolation mode, the workpiece coordinate system can be shifted. The current position display function shows the position viewed from the workpiece coordinate system before the shift. The function to shift the coordinate system is enabled when bit 2 (PLS) of parameter No. 5450 is specified accordingly. The shift can be specified in the polar coordinate interpolation mode, by specifying the position of the center of the rotary axis C (A, B) in the X-C (Y-A, Z-B) interpolation plane with reference to the origin of the workpiece coordinate system, in the following format.

G12.1 X_ C_ ; (Polar coordinate interpolation for the X-axis and C-axis) G12.1 Y_ A_ ; (Polar coordinate interpolation for the Y-axis and A-axis) G12.1 Z_ B_ ; (Polar coordinate interpolation for the Z-axis and B-axis)

G12.1 Xx Cc ;

Center of C-axis

Origin of workpiece coordinate system

Limitation

- Changing the coordinate system during polar coordinate interpolation

In the G12.1 mode, the coordinate system must not be changed (G92, G52, G53, relative coordinate reset, G54 through G59, etc.).

- 19 -

3.INTERPOLATION FUNCTION PROGRAMMING B-64604EN-1/01

- Tool radius/tool nose radius compensation

The polar coordinate interpolation mode (G12.1 or G13.1) cannot be started or terminated in the tool radius/tool nose radius compensation mode (G41 or G42). G12.1 or G13.1 must be specified in the tool radius/tool nose radius compensation canceled mode (G40). For the tool radius/tool nose radius compensation canceled mode (G40) command, be sure to specify the polar coordinate axis to cancel the offset vector. If the polar coordinate interpolation mode (G12.1 or G13.1) is switched without canceling the offset vector, the alarm PS0037, “CAN NOT CHANGE PLANE IN G41/G42” is occurred.

- Tool offset command

A tool offset must be specified before the G12.1 mode is set. No offset can be changed in the G12.1 mode.

- Program restart

For a block in the G12.1 mode, the program and the block cannot be restarted.

- Cutting feedrate for the rotary axis

Polar coordinate interpolation converts the tool movement for a figure programmed in a Cartesian coordinate system to the tool movement in the rotary axis (C-axis) and the linear axis (X-axis). When the tool comes close to the center of the workpiece, the C-axis velocity component increases. If the maximum cutting feedrate for the C-axis (parameter No. 1430) is exceeded, the automatic feedrate override function and automatic speed clamp function are enabled. If the maximum cutting feedrate for the X-axis is exceeded, the automatic feedrate override function and automatic speed clamp function are enabled.

- 20 -

B-64604EN-1/01 PROGRAMMING 3.INTERPOLATION FUNCTION

WARNING

1 Consider lines L1, L2, and L3. ΔX is the distance the tool moves per time unit at

the feedrate specified with address F in the Cartesian coordinate system. As the tool moves from L1 to L2 to L3, the angle at which the tool moves per time unit corresponding to ΔX in the Cartesian coordinate system increases from θ1 to θ2 to θ3. In other words, the C-axis component of the feedrate becomes larger as the tool moves closer to the center of the workpiece. The C component of the feedrate may exceed the maximum cutting feedrate for the C-axis because the tool movement in the Cartesian coordinate system has been converted to the tool movement for the C-axis and the X-axis.

ΔX

L: Distance (in mm) between the tool center and workpiece center when the

tool center is the nearest to the workpiece center

R: Maximum cutting feedrate (deg/min) of the C axis

Then, a speed specifiable with address F in polar coordinate interpolation can be

given by the formula below. If the maximum cutting feedrate for the C-axis is exceeded, the automatic speed control function for polar coordinate interpolation automatically controls the feedrate.

F < L × R ×

(mm/min)

180

- Automatic speed control for polar coordinate interpolation

If the velocity component of the rotary axis exceeds the maximum cutting feedrate in the polar coordinate interpolation mode, the speed is automatically controlled.

- Automatic override

If the velocity component of the rotary axis exceeds the permissible velocity (maximum cutting feedrate multiplied by the permission factor specified in parameter No. 5463), the feedrate is automatically overridden as indicated below. Override = (Permissible velocity) ÷ (Velocity component of rotary axis) × 100(%)

- Automatic speed clamp

If the velocity component of the rotary axis after automatic override still exceeds the maximum cutting feedrate, the speed of the rotary axis is automatically clamped. As a result, the velocity component of the rotary axis will not exceed the maximum cutting feedrate. The automatic speed clamp function works only when the center of the tool is very close to the center of the rotary axis.

- 21 -

3.INTERPOLATION FUNCTION PROGRAMMING B-64604EN-1/01

C-axis

[Example]

G90 G00 X10.0 C0. ; G12.1 ; G01 C0.1 F1000 ; X-10.0 : G13.1 ;

-10.

BCD

+10.

X-axis

Automatic speed control for polar coordinate interpolation

Suppose that the maximum cutting feedrate of the rotary axis is 360 (3600 deg/min) and that the permission factor of automatic override for polar coordinate interpolation (parameter No. 5463) is 0 (90%). If the program indicated above is executed, the automatic override function starts working when the X coordinate becomes 2.273 (point A). The automatic speed clamp function starts working when the X coordinate becomes 0.524 (point B). The minimum value of automatic override for this example is 3%. The automatic speed clamp function continues working until the X coordinate becomes -0.524 (point C). Then, the automatic override function works until the X coordinate becomes -2.273 (point D). (The coordinates indicated above are the values in the Cartesian coordinate system.)

NOTE

1 While the automatic speed clamp function is working, the machine lock or

interlock function may not be enabled immediately.

2 If a feed hold stop is made while the automatic speed clamp function is working,

the automatic operation halt signal *SP is output. However, the operation may not stop immediately.

3 The clamped speed may exceed the clamp value by a few percent.

- 22 -

B-64604EN-1/01 PROGRAMMING 3.INTERPOLATION FUNCTION

Example

Sample program for polar coordinate interpolation in a Cartesian coordinate system consisting of the X-axis (a linear axis) and a hypothetical axis

Hypothetical axis

N204

N205

N206

C axis

N203

N202

N208

N207

Path after cutter compensation

Path before cutter compensation

N201

N200

Tool

Z axis

X axis

O0001; . N010 T0101 . N0100 G90 G00 X60.0 C0 Z

; Positioning to start point N0200 G12.1; Start of polar coordinate interpolation N0201 G42 G01 X20.0F

; N0202 C10.0; N0203 G03 X10.0 C20.0 R10.0; N0204 G01 X-20.0; Geometry program N0205 C-10.0; (program based on cartesian coordinates on N0206 G03 X-10.0 C-20.0 I10.0 J0; X axis-hypothetical axis plane) N0207 G01 X20.0; N0208 C0; N0209 G40 X60.0; N0210 G13.1; Cancellation of polar coordinate interpolation N0300 Z N0400 X

;

C ; . N0900M30;

- 23 -

3.INTERPOLATION FUNCTION PROGRAMMING B-64604EN-1/01

3.2 CONSTANT LEAD THREADING (G32)

Tapered screws and scroll threads in addition to equal lead straight threads can be cut by using a G32 command.

The spindle speed is read from the position coder on the spindle in real time and converted to a cutting feedrate for feed-per minute mode, which is used to move the tool.

Format

G32IP_F_;

F _: Lead of the long axis (always radius programming)

Straight thread

_: End point

Tapered screw

Fig. 3.2 (a) Thread types

X axis

End point_

Scroll thread

Start point

Z axis

Fig. 3.2 (b) Example of threading

Explanation

In general, threading is repeated along the same tool path in rough cutting through finish cutting for a screw. Since threading starts when the position coder mounted on the spindle outputs a one-spindle-rotation signal, threading is started at a fixed point and the tool path on the workpiece is unchanged for repeated threading. Note that the spindle speed must remain constant from rough cutting through finish cutting. If not, incorrect thread lead will occur.

- 24 -

B-64604EN-1/01 PROGRAMMING 3.INTERPOLATION FUNCTION

≤

Tapered thread

45° lead is LZ

lead is LX

α≥45°

Fig. 3.2 (c) LZ and LX of a tapered thread

In general, the lag of the servo system, etc. will produce somewhat incorrect leads at the starting and ending points of a thread cut. To compensate for this, a threading length somewhat longer than required should be specified. Table 3.2 (a) lists the ranges for specifying the thread lead.

Table 3.2 (a) Ranges of lead sizes that can be specified

Least command increment

Metric input 0.0001 to 500.0000 mm

Inch input 0.000001 to 9.999999 inch

- Continuous threading

The "continuous threading" is effective for G32.

- 25 -

3.INTERPOLATION FUNCTION PROGRAMMING B-64604EN-1/01

Example

1. Straight threading

The following values are used in programming :

X axis

2.Tapered threading

X axis

30mm

Zaxis

Thread lead :4mm

Depth of cut :1mm (cut twice) (Metric input, diameter programming)

G00 U-62.0 ; G32 W-74.5 F4.0 ; G00 U62.0 ; W74.5 ; U-64.0 ; (For the second cut, cut 1mm more) G32 W-74.5 ; G00 U64.0 ; W74.5 ;

The following values are used in programming : Thread lead : 3.5mm in the direction of the Z axis

Cutting depth in the X axis direction is 1mm (cut twice) (Metric input, diameter programming) G00 X 12.0 Z72.0 ; G32 X 41.0 Z29.0 F3.5 ; G00 X 50.0 ; Z 72.0 ; X 10.0 ; (Cut 1mm more for the second cut) G32 X 39.0 Z29.0 ; G00 X 50.0 ; Z 72.0 ;

δ δ

=2mm

=1mm

=3mm

=1.5mm

WARNING

1 Feedrate override is effective (fixed at 100%) during threading. 2 It is very dangerous to stop feeding the thread cutter without stopping the

spindle. This will suddenly increase the cutting depth. Thus, the feed hold function is ineffective while threading. If the feed hold button is pressed during threading, the tool will stop after a block not specifying threading is executed as if the SINGLE BLOCK button were pushed. However, the feed hold lamp (SPL lamp) lights when the FEED HOLD button on the machine control panel is pushed. Then, when the tool stops, the lamp is turned off (Single Block stop status).

3 When the FEED HOLD button is pressed again in the first block after threading

mode that does not specify threading (or the button has been held down), the tool stops immediately at the block that does not specify threading.

4 When threading is executed in the single block status, the tool stops after

execution of the first block not specifying threading.

- 26 -

B-64604EN-1/01 PROGRAMMING 3.INTERPOLATION FUNCTION

WARNING

5 When the mode was changed from automatic operation to manual operation

during threading, the tool stops at the first block not specifying threading as when the feed hold button is pushed as mentioned in Warning 3.

However, when the mode is changed from one automatic operation mode to

another, the tool stops after execution of the block not specifying threading as for the single block mode in Note 4.

6 When the previous block was a threading block, cutting will start immediately

without waiting for detection of the one-spindle-rotation signal even if the present block is a threading block.

(Example)

G00 Z0.0 X50.0 ; One-rotation signal is G32 Z10.0 F_ ; : Detected Z20.0 ; : Not detected G32 Z30.0 ; : Not detected

7 Because the constant surface speed control is effective during scroll thread or

tapered screw cutting and the spindle speed changes, the correct thread lead may not be cut. Therefore, do not use the constant surface speed control during threading. Instead, use G97.

8 A movement block preceding the threading block must not specify chamfering or

corner R. 9 A threading block must not specifying chamfering or corner R. 10 The spindle speed override function is disabled during threading. The spindle

speed is fixed at 100%. 11 Thread cycle retract function is ineffective to G32. 12 If tool offset (with the T code or G43.7) is specified in during of the threading

mode, or in a block for threading, alarm PS0509, “TOOL OFFSET COMMAND

IS NOT AVAILABLE”, is issued.

3.3 VARIABLE LEAD THREADING (G34)

Specifying an increment or a decrement value for a lead per screw revolution enables variable lead threading to be performed.

Fig. 3.3 (a) Variable lead screw

NOTE

When bit 1 (NVL) of parameter No.8137 is 0, this function can be used.

- 27 -

3.INTERPOLATION FUNCTION PROGRAMMING B-64604EN-1/01

Format

G34 IP_ F_ K_ Q_ ;

IP_ : End point F_ : Lead in longitudinal axis direction at the start point K_ : Increment and decrement of lead per spindle revolution Q_ : Shift amount of starting angle of thread cutting

Explanation

Address other than K are the same as in straight/taper thread cutting with G32. The K value depends on the increment system of the reference axis, as indicated in Table 3.3 (a). If the specified K value exceeds the range indicated in Table 3.3 (a), if the maximum lead is exceeded after a change due to the K value, or if the lead value is negative, an alarm PS0313, "ILLEGAL LEAD COMMAND", will be issued.

Table 3.3 (a) Range of valid K values

Increment system

of reference axis

IS-A ±0.001 to ±500.000 ±0.00001 to ±50.00000 IS-B ±0.0001 to ±500.0000 ±0.000001 to ±50.000000 IS-C ±0.00001 to ±50.00000 ±0.0000001 to ±5.0000000

Metric input (mm/rev) Inch input (inch/rev)

Table3.3 (b) Range of valid lead values

Metric input (mm) Inch input (inch)

0.0001 to 500.0000 0.000001 to 50.000000

- Continuous threading

The "continuous threading" is effective for G34.

CAUTION

The "thread cutting cycle retract" is not effective for G34.

Example

Lead at the start point: 8.0 mm Lead increment: 0.3 mm/rev G34 Z-72.0 F8.0 K0.3 ;

3.4 CIRCULAR THREADING (G35, G36)

Using the G35 and G36 commands, a circular thread, having the specified lead in the direction of the major axis, can be machined.

L: Lead

Fig. 3.4 (a) Circular threading

- 28 -

B-64604EN-1/01 PROGRAMMING 3.INTERPOLATION FUNCTION

NOTE

This function is an optional function.

Format

A sample format for the G18 plane (Z-X plane) is indicated below. When using the format for the G17 plane (X-Y plane), change the addresses Z, X, K, and I to X, Y, I, and J respectively. When using the format for the G19 plane (Y-Z plane), change the addresses Z, X, K, and I to Y, Z, J, and K respectively.

G35 I_ K_ G36

G35 : Clockwise circular threading command G36 : Counterclockwise circular threading command

X(U), Z(W) : Specify the arc end point (in the same way as for G02, G03).

I, K : Specify the arc center relative to the start point, using relative coordinates (in the

R : Specify the arc radius. F : Specify the lead in the direction of the major axis. Q : Specify the shift of the threading start angle (0° to 360°, with least input increment of 0.001) (The value cannot be programmed with a decimal point.)

X(U)_ Z(W)_

same way as for G02, G03).

F_ Q_ ;

Start point

rc center

Explanation

- Specifying the arc radius

If R is specified with I and K, only R is effective.

- Shift angle

If an angle greater than 360° is programmed, it is set to 360°.

- Continuous threading

The "continuous threading" is effective for G35, G36.

- Thread cutting cycle retract

The "thread cutting cycle retract" is not effective for G35, G36.

End point (Z, X)

- 29 -

3.INTERPOLATION FUNCTION PROGRAMMING B-64604EN-1/01

- Automatic tool compensation

The G36 command is used to specify the following two functions: Automatic tool compensation X and counterclockwise circular threading. The function for which G36 is to be used depends on bit 3 (G36) of parameter No. 3405.

• When parameter G36 is set to 0, the G36 command is used for automatic tool compensation X.

• When parameter G36 is set to 1, the G36 command is used for counterclockwise circular threading.

G37.1 can be used to specify automatic tool compensation X and G37.2 can be used to specify automatic tool compensation Z. (Specification method) G37.1 X_ G37.2 Z_

• G code when bit 3 (G36) of parameter No. 3405 is set to 1

G code G code group Function

G35 Clockwise circular threading G36

G37 Automatic tool compensation Z G37.1 Automatic tool compensation X G37.2

Counterclockwise circular threading

Automatic tool compensation Z

Limitation

- Range of specifiable arc

An arc must be specified such that it falls within a range in which the major axis of the arc is always the Z-axis or always the X-axis, as shown in Fig. 3.4 (b) and Fig. 3.4 (c). If the arc includes a point at which the major axis changes from the X-axis to Z-axis, or vice versa, as shown in Fig. 3.4 (d), an alarm PS5058, "G35/G36 FORMAT ERROR", is issued.

Start point

Fig. 3.4 (b) Range in which the Z-axis is the major axis

End point

45°

Start po int

45°

End point

Fig. 3.4 (c) Range in which the X-axis is the major axis

- 30 -

B-64604EN-1/01 PROGRAMMING 3.INTERPOLATION FUNCTION

Start point

Fig. 3.4 (d) Example of arc specification which causes an alarm

The major axis changes at this point.

End point

- End point not on an arc

If the end point is not on an arc, a movement on an axis is made to a position of which coordinate matches the corresponding coordinate of the end point. Then, a movement is made on another axis to reach the end point.

End point

Center

Start point

Fig. 3.4 (e) Movement when the end point is not on an arc

Start point

Center

3.5 CONTINUOUS THREADING

Threading blocks can be programmed successively to eliminate a discontinuity due to a discontinuous movement in machining by adjacent blocks.

Explanation

Since the system is controlled in such a manner that the synchronism with the spindle does not deviate in the joint between blocks wherever possible, it is possible to performed special threading operation in which the lead and shape change midway.

G32

Fig. 3.5 (a) Continuous threading (Example of G32 in G code system A)

Even when the same section is repeated for threading while changing the depth of cut, this system allows a correct machining without impairing the threads.

G32

- 31 -

3.INTERPOLATION FUNCTION PROGRAMMING B-64604EN-1/01

- Available threading commands

G32: Constant lead threading (G code system A) G33: Constant lead threading (G code system B/C) G34: Variable lead threading G35, G36: Circular threading

- Start angle

The address Q (Angle for shifting the threading start angle) is only effective the first threading command block of continuous threading. In the continuous threading, the addresses Q of the threading in the blocks after the first are ignored.

3.6 MULTIPLE THREADING

Using the Q address to specify an angle between the one-spindle-rotation signal and the start of threading shifts the threading start angle, making it possible to produce multiple-thread screws with ease.

L : Lead

Fig. 3.6 (a) Multiple thread screws.

Format

(Constant lead threading) G32 IP _ F_ Q_ ;

IP : End point F_ : Lead in longitudinal direction

G32 IP _ Q_ ;

Q_ : Angle for shifting the threading start angle (Increment: 0.001 degrees, Valid setting range: 0 to 360 degrees)

Explanation

- Available threading commands

G32: Constant lead threading G34: Variable lead threading G35, G36: Circular threading G76/G78: Multiple threading cycle (Only when the FS10/11 tape format is used.) G92: Threading cycle

Limitation

- Start angle

The start angle is not a continuous state (modal) value. It must be specified each time it is used. If a value is not specified, 0 is assumed.

- Start angle increment

The start angle (Q) increment is 0.001 degrees. Note that no decimal point can be specified. Example:

- 32 -

B-64604EN-1/01 PROGRAMMING 3.INTERPOLATION FUNCTION

For a shift angle of 180 degrees, specify Q180000. Q180.000 cannot be specified, because it contains a decimal point. Note: Q1 is the command of 0.001 degree for the angle for shifting the threading start angle, regardless of

the setting of the followings.

- Increment system IS-A/B/C(Parameter No.1013#1,#0)

- Pocket calculator type decimal point programming (Bit 0(DPI) of parameter No.3401)

- The least input increment is 10 times greater than the least command increment (Bit 7(IPR) of

parameter No.1004)

- Specifiable start angle range

A start angle (Q) of between 0 and 360000 (in 0.001-degree units) can be specified. If a value greater than 360000 (360 degrees) is specified, it is rounded down to 360000 (360 degrees). If a minus value is specified, it works as a plus value. Example: If Q-90000 (-90 degrees) is specified, it works as Q90000 (90 degrees).

- Multiple threading cycle (G76 (G code system A/B)) (G78 (G code system C))

The address Q of the G76/G78 multiple threading cycle command is used for the minimum cutting depth or the depth of cut in 1st cut. For this reason, the angle for shifting the threading start angle can not be commanded. However, if the FS10/11 tape format is used, in G76/G78 multiple threading cycle, the address Q is possible to specify the angle for shifting the threading start angle.

Example

Program for producing double-threaded screws (with start angles of 0 and 180 degrees)

X40.0 ; W-38.0 F4.0 Q0 ; X72.0 ; W38.0 ; X40.0 ; W-38.0 F4.0Q180000 ; X72.0 ; W38.0 ;

- 33 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

4 FUNCTIONS TO SIMPLIFY PROGRAMMING

Chapter 4, "FUNCTIONS TO SIMPLIFY PROGRAMMING", consists of the following sections:

4.1 CANNED CYCLE (G90, G92, G94)..................................................................................................34

4.2 MULTIPLE REPETITIVE CANNED CYCLE (G70-G76)...............................................................52

4.3 CANNED CYCLE FOR DRILLING .................................................................................................91

4.4 RIGID TAPPING..............................................................................................................................106

4.5 CANNED GRINDING CYCLE (FOR GRINDING MACHINE)....................................................119

4.6 CHAMFERING AND CORNER R..................................................................................................129

4.7 MIRROR IMAGE FOR DOUBLE TURRET (G68, G69)...............................................................135

4.8 DIRECT DRAWING DIMENSION PROGRAMMING .................................................................136

4.1 CANNED CYCLE (G90, G92, G94)

There are three canned cycles : the outer diameter/internal diameter cutting canned cycle (G90), the threading canned cycle (G92), and the end face turning canned cycle (G94).

NOTE

1 Explanatory figures in this section use the ZX plane as the selected plane,

diameter programming for the X-axis, and radius programming for the Z-axis. When radius programming is used for the X-axis, change U/2 to U and X/2 to X.

2 A canned cycle can be performed on any plane (including parallel axes for plane

definition). When G-code system A is used, however, U, V, and W cannot be set as a parallel axis.

3 The direction of the length means the direction of the first axis on the plane as

follows: ZX plane: Z-axis direction YZ plane: Y-axis direction XY plane: X-axis direction 4 The direction of the end face means the direction of the second axis on the

plane as follows: ZX plane: X-axis direction YZ plane: Z-axis direction XY plane: Y-axis direction

- 34 -

4.FUNCTIONS TO SIMPLIFY

A’A

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

4.1.1 Outer Diameter/Internal Diameter Cutting Cycle (G90)

This cycle performs straight or taper cutting in the direction of the length.

4.1.1.1 Straight cutting cycle

Format

G90X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.1.1 (a)) in the direction

of the length

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.1.1 (a)) in the

direction of the length

F_ : Cutting feedrate

X axis

4(R)

3(F)

2(F)

Fig. 4.1.1.1 (a) Straight cutting cycle

1(R)

(R)....Rapid traverse

(F)....Cutting fee d

U/2

X/2

Z axis

Explanation

- Operations

A straight cutting cycle performs four operations: (1) Operation 1 moves the tool from the start point (A) to the specified coordinate of the second axis on

the plane (specified X-coordinate for the ZX plane) in rapid traverse.

(2) Operation 2 moves the tool to the specified coordinate of the first axis on the plane (specified

Z-coordinate for the ZX plane) in cutting feed. (The tool is moved to the cutting end point (A') in the direction of the length.)

(3) Operation 3 moves the tool to the start coordinate of the second axis on the plane (start X-coordinate

for the ZX plane) in cutting feed.

(4) Operation 4 moves the tool to the start coordinate of the first axis on the plane (start Z-coordinate for

the ZX plane) in rapid traverse. (The tool returns to the start point (A).)

NOTE

In single block mode, operations 1, 2, 3 and 4 are performed by pressing the

cycle start button once.

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other than G90, G92, or G94.

- 35 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64604EN-1/01

4.1.1.2 Taper cutting cycle

Format

G90 X(U)_Z(W)_R_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.1.2 (a)) in the direction

of the length

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.1.2 (a)) in the

direction of the length R_ : Taper amount (R in the Fig. 4.1.1.2 (a)) F_ : Cutting feedrate

X axis

(R) ....Rapid traverse

4(R)

(F)....Cutting feed

3(F)

U/2

X/2

’

Fig. 4.1.1.2 (a) Taper cutting cycle

2(F)

1(R)

Z axis

Explanation

The figure of a taper is determined by the coordinates of the cutting end point (A') in the direction of the length and the sign of the taper amount (address R). For the cycle in the Fig. 4.1.1.2 (a), a minus sign is added to the taper amount.

NOTE

The increment system of address R for specifying a taper depends on the

increment system for the reference axis. Specify a radius value at R.

- Operations

A taper cutting cycle performs the same four operations as a straight cutting cycle. However, operation 1 moves the tool from the start point (A) to the position obtained by adding the taper amount to the specified coordinate of the second axis on the plane (specified X-coordinate for the ZX plane) in rapid traverse. Operations 2, 3, and 4 after operation 1 are the same as for a straight cutting cycle.

NOTE

In single block mode, operations 1, 2, 3, and 4 are performed by pressing the

cycle start button once.

- Relationship between the sign of the taper amount and tool path

The tool path is determined according to the relationship between the sign of the taper amount (address R) and the cutting end point in the direction of the length in the absolute or incremental programming as Table 4.1.1.2 (a).

- 36 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

Table 4.1.1.2 (a)

Outer diameter machining Intern al diameter machining

1. U < 0, W < 0, R < 0 2. U > 0, W < 0, R > 0

PROGRAMMING

U/2

3(F)

2(F)

4(R)

1(R)

U/2 3(F)

2(F)

4(R)

U/2

3. U < 0, W < 0, R > 0 at |R|≤|U/2|

3(F)

4(R)

2(F)

1(R)

4. U > 0, W < 0, R < 0 at |R|≤|U/2|

U/2

3(F)

2(F)

4(R)

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other than G90, G92, or G94.

1(R)

4.1.2 Threading Cycle (G92)

4.1.2.1 Straight threading cycle

Format

G92 X(U)_Z(W)_F_Q_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.2.1 (a)) in the direction

of the length

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.2.1 (a)) in the

direction of the length Q_ : Angle for shifting the threading start angle (Increment: 0.001 degrees, Valid setting range: 0 to 360 degrees) F_ : Thread lead (L in the Fig. 4.1.2.1 (a))

- 37 -

4. FUNCTIONS TO SIMPLIFY

)

PROGRAMMING

PROGRAMMING B-64604EN-1/01

X axis

3(R

’

4(R)

2(F

1(R

(R) ... Rapid traverse

(F).... Cutting feed

U/2

X/2

Z axis

Approx.

45°

Detailed chamfered thread

Fig. 4.1.2.1 (a) Straight threading

(The chamfered angle in the left figure is 45 degrees or less because of the delay in the servo system.)

Explanation

The ranges of thread leads and restrictions related to the spindle speed are the same as for threading with G32.

- Operations

A straight threading cycle performs four operations: (1) Operation 1 moves the tool from the start point (A) to the specified coordinate of the second axis on

the plane (specified X-coordinate for the ZX plane) in rapid traverse.

(2) Operation 2 moves the tool to the specified coordinate of the first axis on the plane (specified

Z-coordinate for the ZX plane) in cutting feed. At this time, thread chamfering is performed.

(3) Operation 3 moves the tool to the start coordinate of the second axis on the plane (start X-coordinate

for the ZX plane) in rapid traverse. (Retraction after chamfering)

(4) Operation 4 moves the tool to the start coordinate of the first axis on the plane (start Z-coordinate for

the ZX plane) in rapid traverse. (The tool returns to the start point (A).)

CAUTION

Notes on this threading are the same as in threading in G32. However, a stop by

feed hold is as follows; Stop after completion of path 3 of threading cycle.

NOTE

In the single block mode, operations 1, 2, 3, and 4 are performed by pressing

cycle start button once.

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other than G90, G92, or G94.

- Acceleration/deceleration after interpolation for threading

Acceleration/deceleration after interpolation for threading is acceleration/deceleration of exponential interpolation type. By setting bit 5 (THLx) of parameter No. 1610, the same acceleration/deceleration as for cutting feed can be selected. (The settings of bits 1 (CTBx) and 0 (CTLx) of parameter No. 1610 are followed.) However, as a time constant and FL feedrate, the settings of parameter No. 1626 and No. 1627 for the threading cycle are used.

- 38 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

- Time constant and FL feedrate for threading

The time constant for acceleration/deceleration after interpolation for threading specified in parameter No. 1626 and the FL feedrate specified in parameter No. 1627 are used. The FL feedrate is valid only for exponential acceleration/deceleration after interpolation.

- Thread chamfering

Thread chamfering can be performed. A signal from the machine tool, initiates thread chamfering. The chamfering distance r is specified in a range from 0.1L to 12.7L in 0.1L increments by parameter No.

5130. (In the above expression, L is the thread lead.) A thread chamfering angle between 1 to 89 degrees can be specified in parameter No. 5131. When a value of 0 is specified in the parameter, an angle of 45 degrees is assumed. For thread chamfering, the same type of acceleration/deceleration after interpolation, time constant for acceleration/deceleration after interpolation, and FL feedrate as for threading are used.

NOTE

Common parameters for specifying the amount and angle of thread chamfering

are used for this cycle and threading cycle with G76.

- Retraction after chamfering

The Table 4.1.2.1 (a) lists the feedrate, type of acceleration/deceleration after interpolation, and time constant of retraction after chamfering.

Table 4.1.2.1 (a)

Bit 0 (CFR) of

parameter No. 1611

0 Other than 0

0 0

Parameter No.

1466

Description

Uses the type of acceleration/deceleration after interpolation for threading, time constant for threading (parameter No. 1626), FL feedrate (parameter No. 1627), and retraction feedrate specified in parameter No. 1466. Uses the type of acceleration/deceleration after interpolation for threading, time constant for threading (parameter No. 1626), FL feedrate (parameter No. 1627), and rapid traverse rate specified in parameter No. 1420. Before retraction a check is made to see that the specified feedrate has become 0 (delay in acceleration/deceleration is 0), and the type of acceleration/deceleration after interpolation for rapid traverse is used together with the rapid traverse time constant and the rapid traverse rate (parameter No. 1420).

By setting bit 4 (ROC) of parameter No. 1403 to 1, rapid traverse override can be disabled for the feedrate of retraction after chamfering.

NOTE

During retraction, the machine does not stop with an override of 0% for the

cutting feedrate regardless of the setting of bit 4 (RF0) of parameter No. 1401.

- Shifting the start angle

Address Q can be used to shift the threading start angle. The start angle (Q) increment is 0.001 degrees and the valid setting range is between 0 and 360 degrees. No decimal point can be specified.

- 39 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

- Feed hold in a threading cycle (Threading cycle retract)

When feed hold is applied during threading (operation 2), the tool immediately retracts with chamfering and returns to the start point on the second axis (X-axis), then the first axis (Z-axis) on the plane.

X axis

Z axis

Rapid traverse

Cutting feed

Ordinary cycle Motion at feed hold

Start point

Feed hold is effected here.

The chamfered angle is the same as that at the end point.

CAUTION

Another feed hold cannot be made during retreat.

- Inch threading

Inch threading specified with address E is not allowed.

4.1.2.2 Taper threading cycle

Format

G92 X(U)_Z(W)_R_F_Q_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.2.2 (a)) in the direction

of the length

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.2.2 (a)) in the

direction of the length Q_ : Angle for shifting the threading start angle (Increment: 0.001 degrees, Valid setting range: 0 to 360 degrees) R_ : Taper amount (R in the Fig. 4.1.2.2 (a)) F_ : Thread lead (L in the Fig. 4.1.2.2 (a))

- 40 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

X axis

PROGRAMMING

U/2

X/2

’

pprox. 45

3(R)

4(R)

1(R)

2(F)

(The chamfered angle in the left figure is 45 degrees or less because of the delay in the servo system.)

(R)....Rapi d t r averse

(F)....Cutting feed

Z axis

Detailed chamfered thread

Fig. 4.1.2.2 (a) Taper threading cycle

Explanation

The ranges of thread leads and restrictions related to the spindle speed are the same as for threading with G32. The figure of a taper is determined by the coordinates of the cutting end point (A') in the direction of the length and the sign of the taper amount (address R). For the cycle in the Fig. 4.1.2.2 (a), a minus sign is added to the taper amount.

NOTE

The increment system of address R for specifying a taper depends on the

increment system for the reference axis. Specify a radius value at R.

- Operations

A taper threading cycle performs the same four operations as a straight threading cycle. However, operation 1 moves the tool from the start point (A) to the position obtained by adding the taper amount to the specified coordinate of the second axis on the plane (specified X-coordinate for the ZX plane) in rapid traverse. Operations 2, 3, and 4 after operation 1 are the same as for a straight threading cycle.

CAUTION

Notes on this threading are the same as in threading in G32. However, a stop by

feed hold is as follows; Stop after completion of path 3 of threading cycle.

- 41 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64604EN-1/01

NOTE

In the single block mode, operations 1, 2, 3, and 4 are performed by pressing

cycle start button once.

- Relationship between the sign of the taper amount and tool path

Table 4.1.2.2 (a)

Outer diameter machining Intern al diameter machining

1. U < 0, W < 0, R < 0 2. U > 0, W < 0, R > 0

U/2

3(F)

2(F)

4(R)

1(R)

U/2 3(F)

2(F)

4(R)

U/2

3. U < 0, W < 0, R > 0 at |R|≤|U/2|

3(F)

4(R)

2(F)

1(R)

4. U > 0, W < 0, R < 0 at |R|≤|U/2|

U/2

3(F)

2(F)

4(R)

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other than G90, G92, or G94.

- Acceleration/deceleration after interpolation for threading

- Time constant and FL feedrate for threading

- Thread chamfering

- Retraction after chamfering

- Shifting the start angle

- Threading cycle retract

- Inch threading

See the pages on which a straight threading cycle is explained.

1(R)

- 42 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

4.1.3 End Face Turning Cycle (G94)

4.1.3.1 Face cutting cycle

Format

G94 X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.3.1 (a)) in the direction

of the end face

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.3.1 (a)) in the

direction of the end face

F_ : Cutting feedrate

X axis

1(R)

(R)... R apid traverse

(F) .... Cuttin g fe e d

2(F)

U/2

3(F)

’

X/2

Fig. 4.1.3.1 (a) Face cutting cycle

4(R)

Z axis

Explanation

- Operations

A face cutting cycle performs four operations: (1) Operation 1 moves the tool from the start point (A) to the specified coordinate of the first axis on the

plane (specified Z-coordinate for the ZX plane) in rapid traverse.

(2) Operation 2 moves the tool to the specified coordinate of the second axis on the plane (specified

X-coordinate for the ZX plane) in cutting feed. (The tool is moved to the cutting end point (A') in the direction of the end face.)

(3) Operation 3 moves the tool to the start coordinate of the first axis on the plane (start Z-coordinate for

the ZX plane) in cutting feed.

(4) Operation 4 moves the tool to the start coordinate of the second axis on the plane (start X-coordinate

for the ZX plane) in rapid traverse. (The tool returns to the start point (A).)

NOTE

In single block mode, operations 1, 2, 3, and 4 are performed by pressing the

cycle start button once.

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other than G90, G92, or G94.

- 43 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64604EN-1/01

4.1.3.2 Taper cutting cycle

Format

G94 X(U)_Z(W)_R_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.3.2 (a)) in the direction

of the end face

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.3.2 (a)) in the

direction of the end face R_ : Taper amount (R in the Fig. 4.1.3.2 (a)) F_ : Cutting feedrate

X axis

1(R)

U/2

X/2

Fig. 4.1.3.2 (a) Taper cutting cycle

2(F)

’

4(R)

3(F)

(R)... Rap id tra ve rs e (F) ... Cutting feed

Z axis

Explanation

The figure of a taper is determined by the coordinates of the cutting end point (A') in the direction of the end face and the sign of the taper amount (address R). For the cycle in the Fig. 4.1.3.2 (a), a minus sign is added to the taper amount.

NOTE

The increment system of address R for specifying a taper depends on the

increment system for the reference axis. Specify a radius value at R.

- Operations

A taper cutting cycle performs the same four operations as a face cutting cycle. However, operation 1 moves the tool from the start point (A) to the position obtained by adding the taper amount to the specified coordinate of the first axis on the plane (specified Z-coordinate for the ZX plane) in rapid traverse. Operations 2, 3, and 4 after operation 1 are the same as for a face cutting cycle.

NOTE

In single block mode, operations 1, 2, 3, and 4 are performed by pressing the

cycle start button once.

- 44 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

- Relationship between the sign of the taper amount and tool path

The tool path is determined according to the relationship between the sign of the taper amount (address R) and the cutting end point in the direction of the end face in the absolute or incremental programming as Table 4.1.3.2 (a).

Table 4.1.3.2 (a)

Outer diameter machining Intern al diameter machining

1. U < 0, W < 0, R < 0 2. U > 0, W < 0, R < 0

1(R)

U/2

3. U < 0, W < 0, R > 0

U/2

2(F)

at |R|≤|W|

2(F)

3(F)

1(R)

3(F)

4(R)

U/2

2(F)

4. U > 0, W < 0, R > 0 at |R|≤|W|

U/2

2(F)

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other than G90, G92, or G94.

4.1.4 How to Use Canned Cycles (G90, G92, G94)

3(F)

4(R)

1(R)

3(F)

4(R)

1(R)

An appropriate canned cycle is selected according to the shape of the material and the shape of the product.

- Straight cutting cycle (G90)

Shape of material

Shape of product

- 45 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

- Taper cutting cycle (G90)

Shape of material

Shape of product

- Face cutting cycle (G94)

Shape of product

- Face taper cutting cycle (G94)

Shape of material

Shape of product

- 46 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

4.1.5 Canned Cycle and Tool Nose Radius Compensation

When tool nose radius compensation is applied, the tool nose center path and offset direction are as shown below. At the start point of a cycle, the offset vector is canceled. Offset start-up is performed for the movement from the start point of the cycle. The offset vector is temporarily canceled again at the return to the cycle start point and offset is applied again according to the next move command. The offset direction is determined depending of the cutting pattern regardless of the G41 or G42 mode.

Outer diameter/internal diameter cutting cycle (G90)

Tool nose radius center path

Offset direction

Tool nose radius center path

Total tool nose

Programmed path

End face cutting cycle (G94)

Tool nose radius center path

Total tool nose

0 3

Total tool nose

Offset direction

Total tool nose

Programmed path

Total tool nose

Threading cycle (G92)

Tool nose radius compensation cannot be applied.

- 47 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

Differences between this CNC and the FANUC Series 0i-C

NOTE

This CNC is the same as the FANUC Series 0i-C in the offset direction, but

differs from the series in the tool nose radius center path.

- For this CNC Cycle operations of a canned cycle are replaced with G00 or G01. In the first

block to move the tool from the start point, start-up is performed. In the last block to return the tool to the start point, offset is canceled.

- For the FANUC Series 0i-C This series differs from this CNC in operations in the block to move the tool

from the start point and the last block to return it to the start point. For details, refer to "FANUC Series 0i-C Operator's Manual."

How compensation is applied for the FANUC Series 0i-C

G90 G94

Tool nose radius center path

4,8,3

5,0,7

Tool nose radius center path

4,8,3

5,0,7

1,6,2

Total tool

4,5,1

nose

Programmed path

8,0,6

3,7,2

1,6,2

Total tool nose

Programmed path

4,5,1

8,0,6

3,7,2

4.1.6 Restrictions on Canned Cycles

Limitation

- Modal

Since data items X (U), Z (W), and R in a canned cycle are modal values common to G90, G92, and G94. For this reason, if a new X (U), Z (W), or R value is not specified, the previously specified value is effective. Thus, when the travel distance along the Z-axis does not vary as shown in the program example below, a canned cycle can be repeated only by specifying the travel distance along the X-axis.

- 48 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

Example

X axis

The cycle in the above figure is executed by the following program: N030 G90 U-8.0 W-66.0 F0.4; N031 U-16.0; N032 U-24.0; N033 U-32.0;

Workpiece

The modal values common to canned cycles are cleared when a one-shot G code other than G04 is specified. Since the canned cycle mode is not canceled by specifying a one-shot G code, a canned cycle can be performed again by specifying modal values. If no modal values are specified, no cycle operations are performed. When G04 is specified, G04 is executed and no canned cycle is performed.

PROGRAMMING

- Block in which no move command is specified

In a block in which no move command is specified in the canned cycle mode, a canned cycle is also performed. For example, a block containing only EOB or a block in which none of the M, S, and T codes, and move commands are specified is of this type of block. When an M, S, or T code is specified in the canned cycle mode, the corresponding M, S, or T function is executed together with the canned cycle. If this is inconvenient, specify a group 01 G code (G00 or G01) other than G90, G92, or G94 to cancel the canned cycle mode, and specify an M, S, or T code, as in the program example below. After the corresponding M, S, or T function has been executed, specify the canned cycle again.

Example

N003 T0101; : : N010 G90 X20.0 Z10.0 F0.2; N011 G00 T0202;

Cancels the canned cycle mode.

←

N012 G90 X20.5 Z10.0;

- Plane selection command

Specify a plane selection command (G17, G18, or G19) before setting a canned cycle or specify it in the block in which the first canned cycle is specified. If a plane selection command is specified in the canned cycle mode, the command is executed, but the modal values common to canned cycles are cleared. If an axis which is not on the selected plane is specified, alarm PS0330, “ILLEGAL AXIS COMMAND IS IN THE TURNING CANNED CYCLE” is issued.

- Parallel axis

When G code system A is used, U, V, and W cannot be specified as a parallel axis.

- 49 -

4. FUNCTIONS TO SIMPLIFY

)

PROGRAMMING

PROGRAMMING B-64604EN-1/01

- Reset

If a reset operation is performed during execution of a canned cycle when any of the following states for holding a modal G code of group 01 is set, the modal G code of group 01 is replaced with the G01 mode:

• Reset state (bit 6 (CLR) of parameter No. 3402 = 0)

• Cleared state (bit 6 (CLR) of parameter No. 3402 = 1) and state where the modal G code of group 01

is held at reset time (bit 1 (C01) of parameter No. 3406 = 1) Example of operation) If a reset is made during execution of a canned cycle (X0 block) and the X20.Z1. command is

executed, linear interpolation (G01) is performed instead of the canned cycle.

- Manual intervention

After manual intervention is performed with the manual absolute on command before the execution of a canned cycle or after the stop of the execution, when a cycle operation starts, the manual intervention amount is canceled even with an incremental cycle start command.

Example of G94

Cancellation

2(F

3(F)

1(R)

Manual intervention

4(R

- 50 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

4.2 MULTIPLE REPETITIVE CANNED CYCLE (G70-G76)

The multiple repetitive canned cycle is canned cycles to make CNC programming easy. For instance, the data of the finish work shape describes the tool path for rough machining. And also, a canned cycles for the threading is available.

NOTE

1 When bit 3 (NMR) of parameter No.8137 is 0, "Multiple repetitive canned cycle"

can be used. Though, a canned grinding cycle and multiple repetitive canned cycle cannot be used simultaneously. When the canned grinding cycle (the option, "Grinding function A" or "Grinding function B") is enabled, the multiple repetitive canned cycle is disabled.

2 Explanatory figures in this section use the ZX plane as the selected plane,

diameter programming for the X-axis, and radius programming for the Z-axis. When radius programming is used for the X-axis, change U/2 to U and X/2 to X.

3 A multiple repetitive canned cycle can be performed on any plane (including

parallel axes for plane definition). When G-code system A is used, however, U, V, and W cannot be set as a parallel axis.

- 51 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

4.2.1 Stock Removal in Turning (G71)

There are two types of stock removals in turning : Type I and II.

Format

ZpXp plane

G71 U(Δd) R(e) ; G71 P(ns) Q(nf) U(Δu) W(Δw) F(f ) S(s ) T(t ) ;

N (ns) ; ... N (nf) ;

YpZp plane

G71 W(Δd) R(e) ; G71 P(ns) Q(nf) V(Δw) W(Δu) F(f ) S(s ) T(t ) ; N (ns) ; ...

The move commands for the target figure from A to A’ to B are specified in the blocks with sequence numbers ns to nf.

N (nf) ;

XpYp plane

G71 V(Δd) R(e) ; G71 P(ns) Q(nf) U(Δw) V(Δu) F(f ) S(s ) T(t ) ; N (ns) ; ... N (nf) ;

Δd : Depth of cut The cutting direction depends on the direction AA'. This designation is modal and is

not changed until the other value is designated. Also this value can be specified by

the parameter No. 5132, and the parameter is changed by the program command. e : Escaping amount This designation is modal and is not changed until the other value is designated. Also

this value can be specified by the parameter No. 5133, and the parameter is changed

by the program command. ns : Sequence number of the first block for the program of finishing shape. nf : Sequence number of the last block for the program of finishing shape. Δu : Distance of the finishing allowance in the direction of the second axis on the plane

(X-axis for the ZX plane) Δw : Distance of the finishing allowance in the direction of the first axis on the plane (Z-axis

for the ZX plane) f,s,t : Any F , S, or T function contained in blocks ns to nf in the cycle is ignored, and the F,

S, or T function in this G71 block is effective.

Unit Diameter/radius programming Sign

Depends on the increment

Δd

system for the reference axis. Depends on the increment

system for the reference axis.

Radius programming

Not

required

Not

required

Decimal point

input

Allowed

- 52 -

4.FUNCTIONS TO SIMPLIFY

A’Δ

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

Unit Diameter/radius programming Sign

Depends on the increment

Δu

system for the reference axis. Depends on the increment

Δw

system for the reference axis.

Depends on diameter/radius programming for the second axis on the plane. Depends on diameter/radius programming for the first axis on the plane.

Required Allowed

Decimal point

input

(F)

Target figure

(F): Cutting feed (R): Rapid traverse

Fig. 4.2.1 (a) Cutting path in stock removal in turning (type I)

45°

(R)

(F)

e: Escaping amount

u/2

Explanation

- Operations

When a target figure passing through A, A', and B in this order is given by a program, the specified area is removed by Δd (depth of cut), with the finishing allowance specified by Δu/2 and Δw left. After the last cutting is performed in the direction of the second axis on the plane (X-axis for the ZX plane), rough cutting is performed as finishing along the target figure. After rough cutting as finishing, the block next to the sequence block specified at Q is executed.

NOTE

1 While both Δd and Δu are specified by the same address, the meanings of them

are determined by the presence of addresses P and Q. 2 The cycle machining is performed by G71 command with P and Q specification. 3 F, S, and T functions which are specified in the move command between points

A and B are ineffective and those specified in G71 block or the previous block

are effective. M and second auxiliary functions are treated in the same way as F,

S, and T functions. 4 When the constant surface speed control function is enabled (bit 0 (SSC) of

parameter No. 8133 is set to 1), the G96 or G97 command specified in the move

command between points A and B are ineffective, and that specified in G71

block or the previous block is effective.

- Target figure Patterns

The following four cutting patterns are considered. All of these cutting cycles cut the workpiece with moving the tool in parallel to the first axis on the plane (Z-axis for the ZX plane). At this time, the signs of the finishing allowances of Δu and Δw are as follows:

- 53 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64604EN-1/01

Both linear and circular interpolation are possible

U(+)…W(+)

U(-)…W(+)

Fig. 4.2.1 (b) Four target figure patterns

' '

U(+)… W(-)

' '

U(-)…W(-)

Limitation

(1) For U(+), a figure for which a position higher than the cycle start point is specified cannot be

machined.

For U(-), a figure for which a position lower than the cycle start point is specified cannot be

machined.

(2) For type I, the figure must show monotone increase or decrease along the first and second axes on

the plane.

(3) For type II, the figure must show monotone increase or decrease along the first axis on the plane.

- Start block

In the start block in the program for a target figure (block with sequence number ns in which the path between A and A' is specified), G00 or G01 must be specified. If it is not specified, alarm PS0065, “G00/G01 IS NOT IN THE FIRST BLOCK OF SHAPE PROGRAM” is issued. When G00 is specified, positioning is performed along A-A'. When G01 is specified, linear interpolation is performed with cutting feed along A-A'. In this start block, also select type I or II. If X-axis does not move at start block, alarm PS0325 “UNAVAILABLE COMMAND IS IN SHAPE PROGRAM” is issued.

- Check functions

During cycle operation, whether the target figure shows monotone increase or decrease is always checked.

NOTE

When tool nose radius compensation is applied, the target figure to which

compensation is applied is checked.

The following checks can also be made.

Check Related parameter

Checks that a block with the sequence number specified at address Q is contained in the program before cycle operation. Checks the target figure before cycle operation. (Also checks that a block with the sequence number specified at address Q is contained.)

Enabled when bit 2 (QSR) of parameter No. 5102 is set to 1. Enabled when bit 2 (FCK) of parameter No. 5104 is set to 1.

- 54 -

4.FUNCTIONS TO SIMPLIFY

A A

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

- Types I and II Selection of type I or II

For G71, there are types I and II. When the target figure has pockets, be sure to use type II. Escaping operation after rough cutting in the direction of the first axis on the plane (Z-axis for the ZX plane) differs between types I and II. With type I, the tool escapes to the direction of 45 degrees. With type II, the tool cuts the workpiece along the target figure. When the target figure has no pockets, determine the desired escaping operation and select type I or II.

NOTE

To use type II, the multiple repetitive canned cycle II option is required.

Selecting type I or II

In the start block for the target figure (sequence number ns), select type I or II. (1) When type I is selected Specify the second axis on the plane (X-axis for the ZX plane). Do not specify the first axis on the

plane (Z-axis for the ZX plane). (2) When type II is selected Specify the second axis on the plane (X-axis for the ZX plane) and first axis on the plane (Z-axis for

the ZX plane). When you want to use type II without moving the tool along the first axis on the plane (Z-axis for

the ZX plane), specify the incremental programming with travel distance 0 (W0 for the ZX plane).

- Type I

(1) In the block with sequence number ns, only the second axis on the plane (X-axis (U-axis) for the ZX

plane) must be specified.

Example

ZX plane G71 U10.0 R5.0 ;

G71 P100 Q200....;

N100 X(U)_ ;

(Specifies only the second axis on the plane.) : ; : ; N200…………;

(2) The figure along path A'-B must show monotone increase or decrease in the directions of both axes

forming the plane (Z- and X-axes for the ZX plane). It must not have any pocket as shown in the Fig.

4.2.1 (c).

’

Fig. 4.2.1 (c) Figure which does not show monotone increase or decrease (type I)

No pockets are allowed.

- 55 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64604EN-1/01

CAUTION

If a figure does not show monotone change along the first or second axis on the

plane, alarm PS0064, “THE FINISHING SHAPE IS NOT A MONOTONOUS CHANGE(FIRST AXES)” or PS0329, “THE FINISHING SHAPE IS NOT A MONOTONOUS CHANGE(SECOND AXES)” is issued. If the movement does not show monotone change, but is very small, and it can be determined that the movement is not dangerous, however, the permissible amount can be specified in parameters Nos. 5145 and 5146 to specify that the alarm is not issued in this case.

(3) The tool escapes to the direction of 45 degrees in cutting feed after rough cutting.

45°

Fig. 4.2.1 (d) Cutting in the direction of 45 degrees (type I)

Escaping amount e (specified in the command or parameter No. 5133)

(4) Immediately after the last cutting, rough cutting is performed as finishing along the target figure. Bit

1 (RF1) of parameter No. 5105 can be set to 1 so that rough cutting as finishing is not performed.

- Type II

(F)

(R)

(F)

(R)

(F)

Target figure

(F): Cutting feed (R): Rapid traverse

Fig. 4.2.1 (e) Cutting path in stock removal in turning (type II)

’

u/2

When a target figure passing through A, A', and B in this order is given by the program for a target figure as shown in the Fig. 4.2.1 (e), the specified area is removed by Δd (depth of cut), with the finishing allowance specified by Δu/2 and Δw left. Type II differs from type I in cutting the workpiece along the figure after rough cutting in the direction of the first axis on the plane (Z-axis for the ZX plane). After the last cutting, the tool returns to the start point specified in G71 and rough cutting is performed as finishing along the target figure, with the finishing allowance specified by Δu/2 and Δw left.

Type II differs from type I in the following points:

- 56 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

(1) In the block with sequence number ns, the two axes forming the plane (X-axis (U-axis) and Z-axis

(W-axis) for the ZX plane) must be specified. When you want to use type II without moving the tool along the Z-axis on the ZX plane in the first block, specify W0.

PROGRAMMING

Example

ZX plane G71 U10.0 R5.0;

G71 P100 Q200.......;

N100 X(U)_ Z(W)_ ;

(Specifies the two axes forming the plane.) : ; : ; N200…………;

(2) The figure need not show monotone increase or decrease in the direction of the second axis on the

plane (X-axis for the ZX plane) and it may have concaves (pockets).

. . .

Fig. 4.2.1 (f) Figure having pockets (type II)

The figure must show monotone change in the direction of the first axis on the plane (Z-axis for the

ZX plane), however. The Fig. 4.2.1 (g) cannot be machined.

Monotone change is not observed along the Z-

Fig. 4.2.1 (g) Figure which cannot be machined (type II)

axis.

CAUTION

For a figure along which the tool moves backward along the first axis on the

plane during cutting operation (including a vertex in an arc command), the cutting tool may contact the workpiece. For this reason, for a figure which does not show monotone change, alarm PS0064 “THE FINISHING SHAPE IS NOT A MONOTONOUS CHANGE(FIRST AXES)” is issued. If the movement does not show monotone change, but is very small, and it can be determined that the movement is not dangerous, however, the permissible amount can be specified in parameter No. 5145 to specify that the alarm is not issued in this case.

The first cut portion need not be vertical. Any figure is permitted if monotone change is shown in

the direction of the first axis on the plane (Z-axis for the ZX plane).

- 57 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64604EN-1/01

Fig. 4.2.1 (h) Figure which can be machined (type II)

(3) After turning, the tool cuts the workpiece along its figure and escapes in cutting feed.

Escaping amount e (specif ied in the command o parameter No. 5133)

Escaping after cutting

Depth of cut Δd (specified in the command or parameter No. 5132)

Fig. 4.2.1 (i) Cutting along the workpiece figure (type II)

The escaping amount after cutting (e) can be specified at address R or set in parameter No. 5133. When moving from the bottom, however, the tool escapes to the direction of 45 degrees.

45°

e (specified in the command or

parameter No. 5133)

Bottom

Fig. 4.2.1 (j) Escaping from the bottom to the direction of 45 degrees

(4) When a position parallel to the first axis on the plane (Z-axis for the ZX plane) is specified in a

block in the program for the target figure, it is assumed to be at the bottom of a pocket.

(5) After all rough cutting terminates along the first axis on the plane (Z-axis for the ZX plane), the tool

temporarily returns to the cycle start point. At this time, when there is a position whose height equals to that at the start point, the tool passes through the point in the position obtained by adding depth of cut Δd to the position of the figure and returns to the start point.

Then, rough cutting is performed as finishing along the target figure. At this time, the tool passes

through the point in the obtained position (to which depth of cut Δd is added) when returning to the start point.

Bit 2 (RF2) of parameter No. 5105 can be set to 1 so that rough cutting as finishing is not performed.

- 58 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

Escaping operation after rough cutting as finishing

{

Fig. 4.2.1 (k) Escaping operation when the too l returns to the start point (type II)

Escaping operation after rough cutting

Start point

{

Depth of cut Δd

(6) Order and path for rough cutting of pockets Rough cutting is performed in the following order.

(a) When the figure shows monotone decrease along the first axis on the plane (Z-axis for the ZX

plane)

Rough cutting is performed in the order <1>, <2>, and <3> from the rightmost pocket.

<3>

<2>

<1>

Fig. 4.2.1 (l) Rough cutting order in the case of monotone decrease (type II)

(b) When the figure shows monotone increase along the first axis on the plane (Z-axis for the ZX

plane)

Rough cutting is performed in the order <1>, <2>, and <3> from the leftmost pocket.

<1>

Fig. 4.2.1 (m) Rough cutting order in the case of monotone increase (type II)

<2>

<3>

The path in rough cutting is as shown Fig. 4.2.1 (n).

- 59 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

15 7

Fig. 4.2.1 (n) Cutting path for multiple pockets (type II)

The following figure shows how the tool moves after rough cutting for a pocket in detail.

•

Cutting feed

Fig. 4.2.1 (o) Details of motion after cutting for a pocket (type II)

Rapid traverse

Escaping from the bottom

Cuts the workpiece at the cutting feedrate and escapes to the direction of 45 degrees. (Operation 19) Then, moves to the height of point D in rapid traverse. (Operation 20) Then, moves to the position the amount of g before point D. (Operation 21) Finally, moves to point D in cutting feed. The clearance g to the cutting feed start position is set in parameter No. 5134. For the last pocket, after cutting the bottom, the tool escapes to the direction of 45 degrees and returns to the start point in rapid traverse. (Operations 34 and 35)

CAUTION

1 This CNC differs from the FANUC Series 0i-C in cutting of a pocket. The tool first cuts the nearest pocket to the start point. After cutting of the pocket

terminates, the tool moves to the nearest but one pocket and starts cutting.

2 When the figure has a pocket, generally specify a value of 0 for Δw (finishing

allowance). Otherwise, the tool may dig into the wall on one side.

This CNC differs from the FANUC Series 0i-C in the path of cutting after turning depending on the figure of the workpiece. When the tool becomes moving only along the first axis on the plane (Z-axis for the ZX plane) according to the figure of the workpiece during cutting, it starts retraction along the second axis on the plane (X-axis for the ZX plane). When bit 0 (R16) of parameter No. 5108 is set to 1, the cutting can be continued along the first axis on the plane. The cutting path that the target figure program of Fig. 4.2.1 (n) is executed by the setting of bit 0 (R16) of parameter No. 5108, is shown in Fig. 4.2.1 (p).

- 60 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

Fig. 4.2.1 (p) Cutting path (No.5108#0 is set to 1)

- Tool nose radius compensation

When using tool nose radius compensation, specify a tool nose radius compensation command (G41, G42) before a multiple repetitive canned cycle command (G70, G71, G72, G73) and specify the cancel command (G40) outside the programs (from the block specified with P to the block specified with Q) specifying a target finishing figure. If tool nose radius compensation is specified in the program specifying a target finishing figure, alarm PS0325, “UNAVAILABLE COMMAND IS IN SHAPE PROGRAM”, is issued.

Program example

G42;..............................Specify this command before a multiple repetitive canned cycle command.

G71U1.0R0.5; G71P10Q20; N10G00X0; : N20X50.0;

G40;..............................Specify this command after the program specifying a target finishing figure.

When this cycle is specified in the tool nose radius compensation mode, offset is temporarily canceled during movement to the start point. Start-up is performed in the first block. Offset is temporarily canceled again at the return to the cycle start point after termination of cycle operation. Start-up is performed again according to the next move command. This operation is shown in the Fig. 4.2.1 (q).

Start-up

Offset cancel

Cycle start point

Offset cancel

Start-up

Fig. 4.2.1 (q)

- 61 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64604EN-1/01

This cycle operation is performed according to the figure determined by the tool nose radius compensation path when the offset vector is 0 at start point A and start-up is performed in a block between path A-A'.

Position between A-

Target figure program for which tool nose radius compensation is not applied

' in which start-up is

performed

Fig. 4.2.1 (r) Path when tool nose radiu s compensation is applied

Tool nose center pa th when tool nose radius compensation is applied with G42

’

Position between

Target figure program for which tool nose radius

compensation is not applied

Fig. 4.2.1 (s)

Tool nose center pa th when tool nose radius compensation is applied with G42

-A' in which start-

up is performed

NOTE

To perform pocketing in the tool nose radius compensation mode, specify the

linear block A-A' outside the workpiece and specify the figure of an actual pocket. This prevents a pocket from being dug.

When the bit 2 (NT1) of parameter No. 5106 is set to 1, the tool nose radius compensation G40/G41/G42 commanded in the target figure program of the multiple repetitive cycle G71/G72/G73 is ignored and no alarm is occurred.

When the bit 3 (NT2) of parameter No. 5106 is set to 1, the tool nose radius compensation commanded in the target figure program of the multiple repetitive cycle G70 is valid. However there is following limitations. (1) The tool nose radius compensation cancel G40 is selected as the modal when the finishing cycle G70

is commanded.

If the tool nose radius compensation is commanded in the target figure program when G41/G42 is

selected as the modal at the finishing cycle G70 command, the alarm PS0325 “UNAVAILABLE COMMAND IS IN SHAPE PROGRAM” is occurred.

- 62 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

(2) Do not command G41/G42 excluding the end block in the target figure program. If G41 or G42 is specified at the last block of the target figure program, the PS0325 alarm

(UNAVAILABLE COMMAND IS IN SHAPE PROGRAM) is issued. (3) Command G40 at the last block of the target figure program (commanded by Q address) If G40 is not commanded at the last block of the target figure program when G41 or G42 is

commanded at the first block, the PS0538 alarm “OFFSET IS NOT CANCELED” is occurred.

Program example of the tool nose radius compensation in the target figure of G70) G40 ; G70 P10 Q20 ... ; N10 G41 ... ; : N20 G40 ... ;

PROGRAMMING

- Reducing the cycle time

In the multiple repetitive cycle G71/G72 of typeⅠ, if bit 1 (DTP) of parameter No. 5108 is set to 1, the tool return to the cycle start point directly from the end point of the finishing program after rough cutting of the finishing shape program is finished.

Cycle start point ＋

Path of DTP = 0

Distance of the finishing allowance

Path of DTP = 1

End point of finishing shape

Cycle start point

Fig. 4.2.1 (t) Return to cycle start point

In the multiple repetitive cycle G71/G72 of type II, when bit 3 (NSP) of parameter No. 5108 is set to 1, the cutting is executed not to repeat the same cutting path. (When bit 3 (NSP) of parameter No. 5108 is set to 1, the operation of bit 0 (R16) of parameter No. 5108 = 1 is always selected.)

- Case of target figure without pocket. In the conventional method, the path AB is cut twice as Fig. 4.2.1 (w). When bit 3 (NSP) of parameter No. 5108 is set to 1, the overlap is avoided as Fig. 4.2.1(x).

A B

Fig. 4.2.1 (u) Target figure without pocket (No.5108#3=0)

- 63 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

A B

Fig. 4.2.1 (v) Target figure without pocket (No.5108#3=1)

- Case of target figure with pocket. In the conventional method, the path AB and CD are cut twice as Fig. 4.2.1 (y). The cutting path when bit 3 (NSP) of parameter No. 5108 is set to 1 is shown in Fig. 4.2.1(z). The

path AB is overlapped as same as Fig. 4.2.1 (y), however the path AB is executed by rapid traverse at second times. The overlap path CD is avoided.

(3)

(4)

A B

(2)

(1)

Fig. 4.2.1 (w) Targ et fig u re with pocket (No.5108#3=0)

(3)

(4)

A B

(2)

(1)

Fig. 4.2.1 (x) Target figure with pocket (No.5108#3=1)

- Case of consecutive pockets In the conventional method, the tool moves to point I after finish the cutting of a pocket and

positioning to the start point of a next pocket as Fig. 4.2.1 (aa). In this way, the path is overlapped at BI, DI, FI and HI.

The cutting path when bit 3 (NSP) of parameter No. 5108 is set to 1 is shown in Fig. 4.2.1(bb). The

movement to point I is executed just first time and then the pocket cutting is executed one after another.

H I

Fig. 4.2.1 (y) Consecutive pockets (No.5108#3=0)

F G

AB C

- 64 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

H I

Fig. 4.2.1 (z) Consecutive pockets (No.5108#3=1)

F G

AB C

- 65 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

4.2.2 Stock Removal in Facing (G72)

This cycle is the same as G71 except that cutting is performed by an operation parallel to the second axis on the plane (X-axis for the ZX plane).

Format

ZpXp plane

G72 W(Δd) R(e) ; G72 P(ns) Q(nf) U(Δu) W(Δw) F(f ) S(s ) T(t ) ;

N (ns) ; ... N (nf) ;

YpZp plane

G72 V(Δd) R(e) ; G72 P(ns) Q(nf) V(Δw) W(Δu) F(f ) S(s ) T(t ) ; N (ns) ;

The move commands for the target figure from A to A’ to B are specified in the blocks with sequence numbers ns to nf.

... N (nf) ;

XpYp plane

G72 U(Δd) R(e) ; G72 P(ns) Q(nf) U(Δw) V (Δu) F(f ) S(s ) T(t ) ; N (ns) ; ... N (nf) ;

Δd : Depth of cut The cutting direction depends on the direction AA'. This designation is modal and is not

changed until the other value is designated. Also this value can be specified by the

parameter No. 5132, and the parameter is changed by the program command. e : Escaping amount This designation is modal and is not changed until the other value is designated. Also

this value can be specified by the parameter No. 5133, and the parameter is changed

(X-axis for the ZX plane) Δw : Distance of the finishing allowance in the direction of the first axis on the plane (Z-axis

for the ZX plane) f,s,t : Any F , S, or T function contained in blocks ns to nf in the cycle is ignored, and the F, S,

or T function in this G72 block is effective.

Unit Diameter/radius programming Sign

Depends on the increment

Δd

system for the reference axis. Depends on the increment

system for the reference axis.

Radius programming

Not

required

Not

required

Decimal point

input

Allowed

- 66 -

4.FUNCTIONS TO SIMPLIFY

A'Δ

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

Unit Diameter/radius programming Sign

Depends on the increment

Δu

system for the reference axis. Depends on the increment

Δw

system for the reference axis.

Depends on diameter/radius programming for the second axis on the plane. Depends on diameter/radius programming for the first axis on the plane.

Required Allowed

Decimal point

input

(F)

(R)

Target figure

Fig. 4.2.2 (a) Cutting path in stock removal in facing (type I)

(F)

Δw

(F): Cutting feed (R): Rapid traverse

Tool path

(R)

45°

u/2

Explanation

- Operations

NOTE

1 While both Δd and Δu are specified by the same address, the meanings of them

are determined by the presence of addresses P and Q. 2 The cycle machining is performed by G72 command with P and Q specification. 3 F, S, and T functions which are specified in the move command between points

A and B are ineffective and those specified in G72 block or the previous block

are effective. M and second auxiliary functions are treated in the same way as F,

S, and T functions. 4 When the constant surface speed control function is enabled (bit 0 (SSC) of

parameter No. 8133 is set to 1), G96 or G97 command specified in the move

command between points A and B are ineffective, and that specified in G72

block or the previous block is effective.

- Target figure Patterns

The following four cutting patterns are considered. All of these cutting cycles cut the workpiece with moving the tool in parallel to the second axis on the plane (X-axis for the ZX plane). At this time, the signs of the finishing allowances of Δu and Δw are as follows:

- 67 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64604EN-1/01

U(-)...W(+)...

U(-)...W(-)...

' '

U(+)...W(+)...

Fig. 4.2.2 (b) Signs of the values specified at U and W in stock removal in facing

' '

U(+)...W(-)...

Both linear and circular interpolation are possible

Limitation

(1) For W(+), a figure for which a position higher than the cycle start point is specified cannot be

machined.

For W(-), a figure for which a position lower than the cycle start point is specified cannot be

machined.

(2) For type I, the figure must show monotone increase or decrease along the first and second axes on

the plane.

(3) For type II, the figure must show monotone increase or decrease along the second axis on the plane.

- Start block

In the start block in the program for a target figure (block with sequence number ns in which the path between A and A' is specified), G00 or G01 must be specified. If it is not specified, alarm PS0065, “G00/G01 IS NOT IN THE FIRST BLOCK OF SHAPE PROGRAM” is issued. When G00 is specified, positioning is performed along A-A’. When G01 is specified, linear interpolation is performed with cutting feed along A-A’. In this start block, also select type I or II. If Z-axis does not move at start block, alarm PS0325 “UNAVAILABLE COMMAND IS IN SHAPE PROGRAM” is issued.

- Check functions

During cycle operation, whether the target figure shows monotone increase or decrease is always checked.

NOTE

When tool nose radius compensation is applied, the target figure to which

compensation is applied is checked.

The following checks can also be made.

Check Related parameter

Enabled when bit 2 (QSR) of parameter No. 5102 is set to 1. Enabled when bit 2 (FCK) of parameter No. 5104 is set to 1.

- 68 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

- Types I and II Selection of type I or II

For G72, there are types I and II. When the target figure has pockets, be sure to use type II. Escaping operation after rough cutting in the direction of the second axis on the plane (X-axis for the ZX plane) differs between types I and II. With type I, the tool escapes to the direction of 45 degrees. With type II, the tool cuts the workpiece along the target figure. When the target figure has no pockets, determine the desired escaping operation and select type I or II.

Selecting type I or II

In the start block for the target figure (sequence number ns), select type I or II. (1) When type I is selected Specify the first axis on the plane (Z-axis for the ZX plane). Do not specify the second axis on the

plane (X-axis for the ZX plane). (2) When type II is selected Specify the second axis on the plane (X-axis for the ZX plane) and first axis on the plane (Z-axis for

the ZX plane). When you want to use type II without moving the tool along the second axis on the plane (X-axis for

the ZX plane), specify the incremental programming with travel distance 0 (U0 for the ZX plane).

- Type I

G72 differs from G71 in the following points: (1) G72 cuts the workpiece with moving the tool in parallel with the second axis on the plane (X-axis on

the ZX plane). (2) In the start block in the program for a target figure (block with sequence number ns), only the first

axis on the plane (Z-axis (W-axis) for the ZX plane) must be specified.

- Type II

G72 differs from G71 in the following points: (1) G72 cuts the workpiece with moving the tool in parallel with the second axis on the plane (X-axis on

the ZX plane). (2) The figure need not show monotone increase or decrease in the direction of the first axis on the

plane (Z-axis for the ZX plane) and it may have concaves (pockets). The figure must show

monotone change in the direction of the second axis on the plane (X-axis for the ZX plane),

however. (3) When a position parallel to the second axis on the plane (X-axis for the ZX plane) is specified in a

block in the program for the target figure, it is assumed to be at the bottom of a pocket. (4) After all rough cutting terminates along the second axis on the plane (X-axis for the ZX plane), the

tool temporarily returns to the start point. Then, rough cutting as finishing is performed.

- Tool nose radius compensation

See the pages on which G71 is explained.

- Reducing the cycle time

See the pages on which G71 is explained.

- 69 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

4.2.3 Pattern Repeating (G73)

This function permits cutting a fixed pattern repeatedly, with a pattern being displaced bit by bit. By this cutting cycle, it is possible to efficiently cut work whose rough shape has already been made by a rough machining, forging or casting method, etc.

Format

ZpXp plane

G73 W(Δk) U(Δi) R(d) ; G73 P(ns) Q(nf) U(Δu) W(Δw) F(f ) S(s ) T(t ) ;

N (ns) ;

...

N (nf) ;

YpZp plane

G73 V(Δk) W(Δi) R(d) ; G73 P(ns) Q(nf) V(Δw) W(Δu) F(f ) S(s ) T(t ) ; N (ns) ; ... N (nf) ;

XpYp plane

G73 U(Δk) V(Δi) R(d) ; G73 P(ns) Q(nf) U(Δw) V(Δu) F(f ) S(s ) T(t ) ; N (ns) ; ... N (nf) ;

Δi : Distance of escape in the direction of the second axis on the plane (X-axis for the ZX

plane)

This designation is modal and is not changed until the other value is designated. Also

this value can be specified by the parameter No. 5135, and the parameter is changed by the program command.

Δk : Distance of escape in the direction of the first axis on the plane (Z-axis for the ZX

plane)

This designation is modal and is not changed until the other value is designated. Also

this value can be specified by the parameter No. 5136, and the parameter is changed

by the program command. d : The number of division This value is the same as the repetitive count for rough cutting. This designation is

modal and is not changed until the other value is designated. Also, this value can be

specified by the parameter No. 5137, and the parameter is changed by the program

command. ns : Sequence number of the first block for the program of finishing shape. nf : Sequence number of the last block for the program of finishing shape. Δu : Distance of the finishing allowance in the direction of the second axis on the plane

(X-axis for the ZX plane) Δw : Distance of the finishing allowance in the direction of the first axis on the plane (Z-axis

for the ZX plane) f, s, t : Any F, S, and T function contained in the blocks between sequence number "ns" and

"nf" are ignored, and the F, S, and T functions in this G73 block are effective.

The move commands for the target figure from A to A’ to B are specified in the blocks with sequence numbers ns to nf.

- 70 -

4.FUNCTIONS TO SIMPLIFY

Δi+Δ

Δk+Δ

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

Unit Diameter/radius programming Sign

Depends on the increment

Δi

system for the reference axis. Depends on the increment

Δk

system for the reference axis. Depends on the increment

Δu

system for the reference axis. Depends on the increment

Δw

system for the reference axis.

Radius programming Required Allowed

Radius programming Required Allowed Depends on diameter/radius programming for

the second axis on the plane. Depends on diameter/radius programming for the first axis on the plane.

Required Allowed

Decimal point

input

NOTE

Decimal point input is allowed with d. However, a value rounded off to an integer

is used as the number of division, regardless of the setting of bit 0 (DPI) of parameter No. 3401. When an integer is input, the input integer is used as the number of division.

Δw

(R)

(F)

u/2

Δu/2

(R)

Δu/2

' Δw

Target figure

Fig. 4.2.3 (a) Cutting path in pattern repeating

(F): Cutting feed (R): Rapid traverse

Explanation

- Operations

When a target figure passing through A, A', and B in this order is given by a program, rough cutting is performed the specified number of times, with the finishing allowance specified by Δu/2 and Δw left.

NOTE

1 While the values Δi and Δk, or Δu and Δw are specified by the same address

respectively, the meanings of them are determined by the presence of

addresses P and Q. 2 The cycle machining is performed by G73 command with P and Q specification. 3 After cycle operation terminates, the tool returns to point A. 4 F, S, and T functions which are specified in the move command between points

A and B are ineffective and those specified in G73 block or the previous block

are effective. M and second auxiliary functions are treated in the same way as F,

S, and T functions.

- 71 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

- Target figure Patterns

As in the case of G71, there are four target figure patterns. Be careful about signs of Δu, Δw, Δi, and Δk when programming this cycle.

- Start block

In the start block in the program for the target figure (block with sequence number ns in which the path between A and A' is specified), G00 or G01 must be specified. If it is not specified, alarm PS0065, “G00/G01 IS NOT IN THE FIRST BLOCK OF SHAPE PROGRAM” is issued. When G00 is specified, positioning is performed along A-A’. When G01 is specified, linear interpolation is performed with cutting feed along A-A’.

- Check function

The following check can be made.

Check Related parameter

Checks that a block with the sequence number specified at address Q is contained in the program before cycle operation.

Enabled when bit 2 (QSR) of parameter No. 5102 is set to 1.

- Tool nose radius compensation

Like G71, this cycle operation is performed according to the figure determined by the tool nose radius compensation path when the offset vector is 0 at start point A and start-up is performed in a block between path A-A'.

- Single block operation

The single block stop position can be selected by setting of bit 2 (PRS) of parameter No. 5125. When bit 2 (PRS) of parameter No. 5125 is set to 0, the stop position of single block operation are the end point of each cycles and the end point of each blocks in the finishing shape. When bit 2 (PRS) of parameter No. 5125 is set to 1, the stop position of single block operation are the end point of each cycles and the end point of escape from the cycle start point. (FS16i compatible specification)

It explains that the movement when the O0001 shown in Fig. 4.2.3 (b) is executed by the single block operation. The finishing shape specified by N10-N30 of the O0001 is shown in Fig. 4.2.3 (c).

O0001; G00X100.0Z0.0; G73U6.0W6.0R3.0; G73P10Q30U6.0W3.0F1.0S500; N10G00X60.0W0.0; N15G01Z-10.0; N20G02X80.0Z-20.0R10.0; N30G01X100.0; M30;

Fig. 4.2.3 (b) Sample program Fig. 4.2.3 (c) Finishing shape of O0001

N30

N10

N20

N15

When bit 2 (PRS) of parameter No. 5125 is set to 0, in case the O0001 is executed by the single block operation, the stop position of single block operation are the end point of each cycles and the end point of each blocks in the finishing shape as shown in Fig. 4.2.3 (d). The single block stop does not executed at the end point of escape from the cycle start point.

- 72 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

When bit 2 (PRS) of parameter No. 5125 is set to 1, in case the O0001 is executed by the single block operation, the stop position of single block operation are the end point of each cycles and the end point of escape from the cycle start point as shown in Fig. 4.2.3 (e).

“S” in following figures stands for the single stop position.

PROGRAMMING

Fig. 4.2.3 (d) PRS(No.5125#2)=0 Fig. 4.2.3 (e) PRS(No.5125#2)=1

- 73 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

4.2.4 Finishing Cycle (G70)

After rough cutting by G71, G72 or G73, the following command permits finishing.

Format

G70 P(ns) Q(nf) ;

ns : Sequence number of the first block for the program of finishing shape. nf : Sequence number of the last block for the program of finishing shape.

Explanation

- Operations

The blocks with sequence numbers ns to nf in the program for a target figure are executed for finishing. The F, S, T, M, and second auxiliary functions specified in the G71, G72, or G73 block are ignored and the F, S, T, M, and second auxiliary functions specified in the blocks with sequence numbers ns to nf are effective. When cycle operation terminates, the tool is returned to the start point in rapid traverse and the next G70 cycle block is read.

- Target figure Check function

The following check can be made.

Check Related parameter

Checks that a block with the sequence number specified at address Q is contained in the program before cycle operation.

- Storing P and Q blocks

When rough cutting is executed by G71, G72, or G73, up to three memory addresses of P and Q blocks are stored. By this, the blocks indicated by P and Q are immediately found at execution of G70 without searching memory from the beginning for them. After some G71, G72, and G73 rough cutting cycles are executed, finishing cycles can be performed by G70 at a time. At this time, for the fourth and subsequent rough cutting cycles, the cycle time is longer because memory is searched for P and Q blocks.

Example

G71 P100 Q200 ...; N100 ...; ...; ...; N200 ...; G71 P300 Q400 ...; N300 ...; ...; ...; N400 ...; ...; ...; G70 P100 Q200 ; (Executed without a search for the first to third cycles) G70 P300 Q400 ; (Executed after a search for the fourth and subsequent

cycles)

Enabled when bit 2 (QSR) of parameter No. 5102 is set to 1.

- 74 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

NOTE

The memory addresses of P and Q blocks stored during rough cutting cycles by

G71, G72, and G73 are erased after execution of G70.

All stored memory addresses of P and Q blocks are also erased by a reset.

- Return to the cycle start point

In a finishing cycle, after the tool cuts the workpiece to the end point of the target figure, it returns to the cycle start point in rapid traverse.

NOTE

The tool returns to the cycle start point always in the nonlinear positioning mode

regardless of the setting of bit 1 (LRP) of parameter No. 1401.

Before executing a finishing cycle for a target figure with a pocket cut by G71 or

G72, check that the tool does not interfere with the workpiece when returning from the end point of the target figure to the cycle start point.

- Tool nose radius compensation

When using tool nose radius compensation, specify a tool nose radius compensation command (G41 or G42) before a multiple repetitive canned cycle command (G70) and specify the cancel command (G40) after the multiple repetitive canned cycle command (G70).

Program example

G42;..............................Specify this command before a multiple repetitive canned cycle command.

G70P10Q20;

G40;..............................Specify this command after a multiple repetitive canned cycle command.

- 75 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

Example

Stock removal in facing (G72)

20 2

Start point

Z axis

X axis

160

120

2010

190

(Diameter designation for X axis, metric input) N010 G50 X220.0 Z190.0 ;

N011 G00 X176.0 Z132.0 ; N012 G72 W7.0 R1.0 ; N013 G72 P014 Q019 U4.0 W2.0 F0.3 S550 ; N014 G00 Z56.0 S700 ; N015 G01 X120.0 W14.0 F0.15 ; N016 W10.0 ; N017 X80.0 W10.0 ; N018 W20.0 ; N019 X36.0 W22.0 ; N020 G70 P014 Q019 ;

Escaping amount: 1.0 Finishing allowance (4.0 in diameter in the X direction, 2.0 in the Z direction)

- 76 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

Pattern repeating (G73)

X axis

PROGRAMMING

180

160

120

220

(Diameter designation, metric input)

N010 G50 X260.0 Z220.0 ; N011 G00 X220.0 Z160.0 ; N012 G73 U14.0 W14.0 R3 ; N013 G73 P014 Q019 U4.0 W2.0 F0.3 S0180 ; N014 G00 X80.0 W-40.0 ; N015 G01 W-20.0 F0.15 S0600 ; N016 X120.0 W-10.0; N017 W-20.0 S0400 ; N018 G02 X160.0 W-20.0 R20.0 ; N019 G01 X180.0 W-10.0 S0280 ; N020 G70 P014 Q019 ;

110

130

Z axis

- 77 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

4.2.5 End Face Peck Drilling Cycle (G74)

This cycle enables chip breaking in outer diameter cutting. If the second axis on the plane (X-axis (U-axis) for the ZX plane) and address P are omitted, operation is performed only along the first axis on the plane (Z-axis for the ZX plane), that is, a peck drilling cycle is performed.

Format

G74R (e) ; G74X(U)_ Z(W)_ P(Δi) Q(Δk) R(Δd) F (f ) ;

e : Return amount This designation is modal and is not changed until the other value is designated.

Also this value can be specified by the parameter No. 5139, and the parameter is

changed by the program command. X_,Z_ : Coordinate of the second axis on the plane (X-axis for the ZX plane) at point B and Coordinate of the first axis on the plane (Z-axis for the ZX plane) at point C U_,W_ : Travel distance along the second axis on the plane (U for the ZX plane) from point A

to B Travel distance along the first axis on the plane (W for the ZX plane) from point A to

C (When G code system A is used. In other cases, X_,Z_ is used for specification.) Δi : Travel distance in the direction of the second axis on the plane (X-axis for the ZX

plane)

Δk : Depth of cut in the direction of the first axis on the plane (Z-axis for the ZX plane) Δd : Relief amount of the tool at the cutting bottom

f : Feedrate

Unit

Depends on the increment system for

the reference axis. Depends on the increment system for

Δi

the reference axis. Depends on the increment system for

Δk

the reference axis. Depends on the increment system for

Δd

the reference axis.

Diameter/radius

programming

Radius programming Not required Allowed

Radius programming Not required Not allowed

Radius programming NOTE Allowed

Sign

NOTE

Normally, specify a positive value for Δd. When X (U) and Δi are omitted, specify

a value with the sign indicating the direction in which the tool is to escape.

Decimal point

input

- 78 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

Δk' Δk

(R)

(F)

Fig. 4.2.5 (a) Cutting path in end face peek drilling cycle

(F)

(R)

Δk

(F)

(R)

Δk

(F)

Δk

(F)

(R)

[0 < Δk’ ≤ Δk]

Δi

(R)

U/2

Δi

Δi’

(R) ... Rapid traverse (F) ... Cutting feed

[0 < Δi’ ≤ Δi]

Explanation

- Operations

A cycle operation of cutting by Δk and return by e is repeated. When cutting reaches point C, the tool escapes by Δd. Then, the tool returns in rapid traverse, moves to the direction of point B by Δi, and performs cutting again.

NOTE

1 While both e and Δd are specified by the same address, the meanings of them

are determined by specifying the X, Y, or Z axis. When the axis is specified, Δd is used.

2 The cycle machining is performed by G74 command with specifying the axis.

- Tool nose radius compensation

Tool nose radius compensation cannot be applied.

- 79 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

4.2.6 Outer Diameter / Internal Diameter Drilling Cycle (G75)

This cycle is equivalent to G74 except that the second axis on the plane (X-axis for the ZX plane) changes places with the first axis on the plane (Z-axis for the ZX plane). This cycle enables chip breaking in end facing. It also enables grooving during outer diameter cutting and cutting off (when the Z-axis (W-axis) and Q are omitted for the first axis on the plane).

Format

G75R (e) ; G75X(U)_ Z(W)_ P(Δi) Q(Δk) R(Δd) F (f ) ;

e : Return amount This designation is modal and is not changed until the other value is designated.

Also this value can be specified by the parameter No. 5139, and the parameter is

changed by the program command. X_, Z_ : Coordinate of the second axis on the plane (X-axis for the ZX plane) at point B and Coordinate of the first axis on the plane (Z-axis for the ZX plane) at point C U_, W_ : Travel distance along the second axis on the plane (U for the ZX plane) from point

A to B Travel distance along the first axis on the plane (W for the ZX plane) from point A

to C (When G code system A is used. In other cases, X_,Z_ is used for specification.) Δi : Depth of cut in the direction of the second axis on the plane (X-axis for the ZX

plane) Δk : Travel distance in the direction of the first axis on the plane (Z-axis for the ZX

plane) Δd : Relief amount of the tool at the cutting bottom f : Feedrate

Unit Diameter/radius programming Sign

Depends on the increment system for

the reference axis. Depends on the increment system for

Δi

the reference axis. Depends on the increment system for

Δk

the reference axis. Depends on the increment system for

Δd

the reference axis.

Radius programming Not required Allowed

Radius programming Not required Not allowed

Radius programming NOTE Allowed

NOTE

Normally, specify a positive value for Δd. When Z (W) and Δk are omitted,

specify a value with the sign indicating the direction in which the tool is to escape.

Decimal point

input

- 80 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

(R)

(F)

Δi

U/2

Δi

Δi’

Δd

(R) ... Rapid traverse (F) ... Cutting feed

Fig. 4.2.6 (b) Outer diameter/internal diameter drilling cycle

Explanation

- Operations

A cycle operation of cutting by Δi and return by e is repeated. When cutting reaches point B, the tool escapes by Δd. Then, the tool returns in rapid traverse, moves to the direction of point C by Δk, and performs cutting again.

Both G74 and G75 are used for grooving and drilling, and permit the tool to relief automatically. Four symmetrical patterns are considered, respectively.

- Tool nose radius compensation

Tool nose radius compensation cannot be applied.

- 81 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

4.2.7 Multiple Threading Cycle (G76)

This threading cycle performs one edge cutting by the constant amount of cut.

Format

G76 P(m) (r) (a) Q(Δdmin) R(d ) ; G76 X(U)_ Z(W)_ R(i ) P(k ) Q(Δd) F (L ) ;

m : Repetitive count in finishing (1 to 99) This value can be specified by the parameter No. 5142, and the parameter is changed by

the program command. r : Chamfering amount (0 to 99) When the thread lead is expressed by L, the value of L can be set from 0.0L to 9.9L in

0.1L increment (2-digit number). This value can be specified by the parameter No. 5130,

and the parameter is changed by the program command. a : Angle of tool nose One of six kinds of angle, 80°, 60°, 55°, 30°, 29°, and 0°, can be selected, and specified

by 2-digit number. This value can be specified by the parameter No. 5143, and the

parameter is changed by the program command.

m, r, and a are specified by address P at the same time.

(Example) When m=2, r=1.2L, a=60°, specify as shown below (L is lead of thread).

P 02 12 60

Δdmin : Minimum cutting depth When the cutting depth of one cycle operation becomes smaller than this limit, the

cutting depth is clamped at this value. This value can be specified by parameter

No. 5140, and the parameter is changed by the program command. d : Finishing allowance This value can be specified by parameter No. 5141, and the parameter is changed

by the program command. X_, Z_ : Coordinates of the cutting end point (point D in the Fig. 4.2.7 (a)) in the direction of

the length U_, W_ : Travel distance to the cutting end point (point D in the Fig. 4.2.7 (a)) in the direction

of the length (When G code system A is used. In other cases, X_,Z_ is used for specification.) i : Taper amount If i = 0, ordinary straight threading can be made. k : Height of thread Δd : Depth of cut in 1st cut L : Lead of thread

Unit

Δdmin

Depends on the increment system for the reference axis. Depends on the increment system for

the reference axis. Depends on the increment system for

the reference axis.

Diameter/radius

programming

Radius programming Not required Not allowed

Radius programming Not required Allowed

Radius programming Required Allowed

Radius programming Not required Not allowed

Sign

Decimal point

input

- 82 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

PROGRAMMING

Unit

Depends on the increment system for

Δd

the reference axis.

U/2

(R)

Fig. 4.2.7 (a) Cutting path in multiple threading cycle

Diameter/radius

programming

Sign

Decimal point

input

Radius programming Not required Not allowed

(R) A

(R)

(F)

Δd

Tool nose

Δd√n

1st

2nd

3rd

nth

Fig. 4.2.7 (b) Detail of cutting

- Repetitive count in finishing

The last finishing cycle (cycle in which the finishing allowance is removed by cutting) is repeated.

- 83 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

Last finishi ng cy c l e

Fig. 4.2.7 (c)

d (finishing allowance)

Explanation

- Operations

This cycle performs threading so that the length of the lead only between C and D is made as specified in the F code. In other sections, the tool moves in rapid traverse. The time constant for acceleration/deceleration after interpolation and FL feedrate for thread chamfering and the feedrate for retraction after chamfering are the same as for thread chamfering with G92 (canned cycle).

NOTE

1 The meanings of the data specified by address P, Q, and R determined by the

presence of X (U) and Z (W).

2 The cycle machining is performed by G76 command with X (U) and Z (W)

specification.

3 The values specified at addresses P, Q, and R are modal and are not changed

until another value is specified.

4 Specify a value smaller than the height of thread as the finishing allowance. (d <

CAUTION

Notes on threading are the same as those on G32 threading. For feed hold in a

threading cycle, however, see "Feed hold in a threading cycle" described below.

- Relationship between the sign of the taper amount and tool path

The signs of incremental dimensions for the cycle shown in Fig. 4.2.7 (a) are as follows: Cutting end point in the direction of the length for U and W: Minus (determined according to the directions of paths A-C and C-D) Taper amount (i): Minus (determined according to the direction of path A-C) Height of thread (k): Plus (always specified with a plus sign) Depth of cut in the first cut (Δd): Plus (always specified with a plus sign) The four patterns shown in the Table 4.2.7 (a) are considered corresponding to the sign of each address. A female thread can also be machined.

- 84 -

4.FUNCTIONS TO SIMPLIFY

B-64604EN-1/01 PROGRAMMING

Table 4.2.7 (a)

Outer diameter machining Intern al diameter machining

1. U < 0, W < 0, i < 0 2. U > 0, W < 0, i > 0

PROGRAMMING

U/2

3(R)

3. U < 0, W < 0, i > 0

3(R)

4(R)

2(F)

at |i|≤|U/2|

4(R)

2(F)

1(R)

U/2 3(R)

4. U > 0, W < 0, i < 0 at |i|≤|U/2|

U/2

3(R)

2(F)

4(R)

2(F)

4(R)

1(R)

- Acceleration/deceleration after interpolation for threading

- Time constant and FL feedrate for threading

- Thread chamfering

Thread chamfering can be performed in this threading cycle. A signal from the machine tool initiates thread chamfering. The maximum amount of thread chamfering (r) that can be specified in the command is 99 (9.9L). The amount can be specified in a range from 0.1L to 12.7L in 0.1L increments in parameter No. 5130. A thread chamfering angle between 1 to 89 degrees can be specified in parameter No. 5131. When a value of 0 is specified in the parameter, an angle of 45 degrees is assumed. For thread chamfering, the same type of acceleration/deceleration after interpolation, time constant for acceleration/deceleration after interpolation, and FL feedrate as for threading are used.

NOTE

Common parameters for specifying the amount and angle of thread chamfering

are used for this cycle and G92 threading cycle.

- 85 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64604EN-1/01

- Retraction after chamfering

The Table 4.2.7 (b) lists the feedrate, type of acceleration/deceleration after interpolation, and time constant of retraction after chamfering.

Table 4.2.7 (b)

Bit 0 (CFR) of

parameter No. 1611

0 Other than 0

0 0

Parameter No.

1466

Description

By setting bit 4 (ROC) of parameter No. 1403 to 1, rapid traverse override can be disabled for the feedrate of retraction after chamfering.

NOTE

During retraction, the machine does not stop with an override of 0% for the

cutting feedrate regardless of the setting of bit 4 (RF0) of parameter No. 1401.

- Shifting the start angle

The threading start angle cannot be shifted. However, if the Series 10/11 format is used, the threading start angle can be shifted. Please refer to the "MEMORY OPERATION USING Series 10/11 FORMAT".

- Feed hold in a threading cycle (threading cycle retract)

When feed hold is applied during threading in a combined threading cycle (G76), the tool quickly retracts in the same way as for the last chamfering in a threading cycle and returns to the start point in the current cycle. When cycle start is triggered, the multiple threading cycle resumes.

X-axis

Z-axis

Ordinary cycle Motion at feed hold

Start point in the current cycle

Rapid traverse

Cu ttin g fe ed

Feed hold is applied at this point

Fig. 4.2.7 (d)

The angle of chamfering during retraction is the same as that of chamfering at the end point.

- 86 -

fanuc 0i- F Operators Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

SAFETY PRECAUTIONS

DEFINITION OF WARNING, CAUTION, AND NOTE

GENERAL WARNINGS AND CAUTIONS

WARNINGS AND CAUTIONS RELATED TO PROGRAMMING

WARNINGS AND CAUTIONS RELATED TO HANDLING

WARNINGS RELATED TO DAILY MAINTENANCE

TABLE OF CONTENTS

I. GENERAL

1 GENERAL

1.2 NOTES ON READING THIS MANUAL

1.3 NOTES ON VARIOUS KINDS OF DATA

II. PROGRAMMING

1 GENERAL

1.1 OFFSET

2 PREPARATORY FUNCTION (G FUNCTION)

3 INTERPOLATION FUNCTION

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

3.2 CONSTANT LEAD THREADING (G32)

3.3 VARIABLE LEAD THREADING (G34)

3.4 CIRCULAR THREADING (G35, G36)

3.5 CONTINUOUS THREADING

3.6 MULTIPLE THREADING

4 FUNCTIONS TO SIMPLIFY PROGRAMMING

4.1 CANNED CYCLE (G90, G92, G94)

4.1.1 Outer Diameter/Internal Diameter Cutting Cycle (G90)

4.1.1.1 Straight cutting cycle

4.1.1.2 Taper cutting cycle

4.1.2 Threading Cycle (G92)

4.1.2.1 Straight threading cycle

4.1.2.2 Taper threading cycle

4.1.3 End Face Turning Cycle (G94)

4.1.3.1 Face cutting cycle

4.1.3.2 Taper cutting cycle

4.1.4 How to Use Canned Cycles (G90, G92, G94)

4.1.5 Canned Cycle and Tool Nose Radius Compensation

4.1.6 Restrictions on Canned Cycles

4.2 MULTIPLE REPETITIVE CANNED CYCLE (G70-G76)

4.2.1 Stock Removal in Turning (G71)

4.2.2 Stock Removal in Facing (G72)

4.2.3 Pattern Repeating (G73)

4.2.4 Finishing Cycle (G70)

4.2.5 End Face Peck Drilling Cycle (G74)

4.2.6 Outer Diameter / Internal Diameter Drilling Cycle (G75)

4.2.7 Multiple Threading Cycle (G76)