fanuc 0i-F Plus Operator’s Manual

Download

Page 1

< Series 0+-MODEL F Plus

For Lathe System

OPERATOR'S MANUAL

B-64694EN-1/01

Page 2

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

Foreign Exchange and

The export from Japan may be subject to an export license by the

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

to safety.

regarded as “impossible”.

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

The products in this manual are controlled based on Japan’s “ Foreign Trade Law”. government of Japan. 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.

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

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

Page 3

B-64694EN-1/01 SAFETY PRECAUTIONS

SAFETY PRECAUTION

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.

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

Used if a danger resulting in the death or serious injury of the user is expected to

occur if he or she fails to observe the approved procedure.

CAUTION

Used if a danger resulting in the minor or moderate injury of the user or

equipment damage is expected to occur if he or she fails to observe the approved procedure.

NOTE

Used if a supplementary explanation not related to any of WARNING, and

CAUTION is to be indicated.

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

s-1

Page 4

SAFETY PRECAUTIONS B-64694EN-1/01

WARNING

or injury to the user.

GENERAL WARNINGS AND CAUTIONS

1 Never attempt to machine a workpiece without first checking the operation of the

2 Before operating the machine, thoroughly check the entered data. Operating the machine with incorrectly specified data may result in the machine

3 Ensure that the specified feedrate is appropriate for the intended operation. The appropriate feedrate varies with the intended operation. Refer to the manual If a machine is run at other than the correct speed, it may behave unexpectedly,

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

5 The parameters for the CNC and PMC are factory-set. Usually, there is not need

Failure to set a parameter correctly may result in the machine behaving

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 m achine may result in the machine behaving unexpectedly, possibly causing damage to the workpiece and/or machine itself, or injury to the user.

behaving unexpectedly, possibly causing damage to the workpiece and/or machine itself, or injury to the user.

Generally, for each machine, there is a maximum allowable feedrate. provided with the machine to determine the maximum allowable feedrate. possibly causing damage to the workpiece and/or machine itself, or injury to the

user. 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.

to change them. When, however, there is not alternative other than to change a parameter, ensure that you fully understand the function of the param et er before making any change.

unexpectedly, possibly causing damage to the workpiece and/or machine itself,

s-2

Page 5

B-64694EN-1/01 SAFETY PRECAUTIONS

CAUTION

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

unexpectedly.

2 The OPERATOR’S MANUAL and programming manual supplied with a CNC

machine if in doubt.

3 Some functions may have been implemented at the request of the machine-tool

machine-tool builder for details of their use and any related cautions.

4 The liquid-crystal display is manufactured with very precise fabrication

phenomenon is a common attribute of LCDs and is not a defect.

NOTE

non-volatile memory at registration, modification, or deletion of program s.

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

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

builder. When using such functions, refer to the manual supplied by the

technology. Some pixels may not be turned on or may remain on. This

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. 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 t he

s-3

Page 6

SAFETY PRECAUTIONS B-64694EN-1/01

WARNING

Coordinate system setting

damage the tool, the machine itself, the workpiece, or cause injury to the user .

Inch/metric conversion

to the user.

Constant surface speed control

machine itself, the workpiece, or cause injury to the user.

Stroke check

workpiece, or causing injury to the user.

WARNINGS AND CAUTIONS RELATED TO PROGRAMM ING

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 f amiliar with their contents.

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 caref ully confirmed before performing programming. Positioning involves rapid travers e. 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 rotat ion 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

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 measur ement 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

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

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

s-4

Page 7

B-64694EN-1/01 SAFETY PRECAUTIONS

WARNING

7 I

nterference check for each path

automatic operation and specify the tool number of the tool to be used.

Same address command in same block

program command”）

CAUTION

Absolute/incremental mode

versa, the machine may behave unexpectedly.

Plane selection

descriptions of the respective functions for details.

Torque limit skip

be executed without performing a skip.

Programmable mirror image

mirror image is enabled.

Compensation function

compensation function mode.

Interference check for each path function is perform ed bas ed on t he 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

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 t he m ac hine 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

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

If an incorrect plane is specified for circular interpolation, helical interpolation, or

a canned cycle, the machine may behave unexpectedly. Refer to the

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

Note that programmed operations vary considerably when a programmable

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

s-5

Page 8

SAFETY PRECAUTIONS B-64694EN-1/01

WARNING

Manual operation

injury to the user.

Workpiece coordinate system shift

workpiece, or causing injury to the operator.

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.

When operating the machine manually, determine the current position of the tool

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

3 In manual handle feed, rotating the handle with a large scale factor, such as 100,

4 If override is disabled (according to the specification in a macro variable) during

5 Basically, never attempt an origin/preset operation when the machine is

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

required. If the machine is operated without first performing manual reference posit ion 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 handle feed

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

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

operating under the control of a program. Otherwise, the machine may behave unexpectedly, possibly damaging the tool, the machine itself, the tool, or causing

Manual intervention, machine lock, or mirror imaging may shift the workpiece

coordinate system. Before attempting to operate the machine under the c ont rol 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

s-6

Page 9

B-64694EN-1/01 SAFETY PRECAUTIONS

WARNING

Software operator's panel and menu switches

use the emergency stop button instead of the RESET key to ensure security.

CAUTION

Manual intervention

command mode.

Feed hold, override, and single block

machine in this case.

Dry run

sometimes be higher than the programmed feed rate.

Program editing

modify, insert, or delete commands from a machining program while it is in use.

PS alarm

the axis movement stops.

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,

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, c onf ir m the settings of the manual absolute switches, parameters, and absolute/incremental

The feed hold, feedrate override, and single block functions can be disabled

using custom macro system variable #3004. Be careful when operating the

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

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

When a PS alarm is occurred during executing a blolck, the axis movement of

the block is continued to the end of block. After finishing the executing the block,

s-7

Page 10

SAFETY PRECAUTIONS B-64694EN-1/01

WARNING

electric shock hazard.

NOTE

replacement procedure.

WARNING

electric shock hazard.

NOTE

details of the battery replacement procedure.

WARNINGS RELATED TO DAILY MAINTENANCE

Memory backup battery replacement

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

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

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

(marked and fitted with an insulating cover).

Touching the uncovered high-voltage circuits presents an extremely dangerous

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 OPERATOR’S

MANUAL (Common to Lathe/Machining Center System) for details of the batter y

Absolute pulse coder 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

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 AMPLIFIER

series Maintenance Manual for

s-8

Page 11

B-64694EN-1/01 SAFETY PRECAUTIONS

WARNING

electric shock hazard.

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

s-9

Page 12

Page 13

B-64694EN-1/01 TABLE OF CONTENTS

SAFETY PRECAUTION .............................................................................. s-1

I. GENERAL

1 GENERAL ............................................................................................... 3

1.1 NOTES ON READING THIS MANUAL .......................................................... 6

1.2 NOTES ON VARIOUS KINDS OF DATA ...................................................... 6

II. PROGRAMMING

1 GENERAL ............................................................................................... 9

1.1 OFFSET ........................................................................................................ 9

2 PREPARATORY FUNCTION (G FUNCTION) ...................................... 10

3 INTERPOLATION FUNCTION .............................................................. 15

3.1 THREADING (G32) ..................................................................................... 15

3.2 CONTINUOUS THREADING ....................................................................... 18

3.3 MULTIPLE THREADING ............................................................................. 19

4 FUNCTIONS TO SIMPLIFY PROGRAMMING ..................................... 21

4.1 CANNED CYCLE (G90, G92, G94) ............................................................. 21

4.1.1 Outer Diameter/Internal Diameter Cutting Cycle (G90) ........................................ 22

4.1.1.1 Straight cutting cycle ......................................................................................... 22

4.1.1.2 Taper cutting cycle ............................................................................................ 23

4.1.2 Threading Cycle (G92) ........................................................................................... 24

4.1.2.1 Straight threading cycle ..................................................................................... 24

4.1.2.2 Taper threading cycle ........................................................................................ 27

4.1.3 End Face Turning Cycle (G94) .............................................................................. 30

4.1.3.1 Face cutting cycle .............................................................................................. 30

4.1.3.2 Taper cutting cycle ............................................................................................ 31

4.1.4 How to Use Canned Cycles (G90, G92, G94) ........................................................ 32

4.1.5 Canned Cycle and Tool Nose Radius Compensation ............................................. 34

4.1.6 Restrictio ns on Canned Cycles ............................................................................... 35

4.2 MULTIPLE REPETITIVE CANNED CYCLE (G70-G76) .............................. 37

4.2.1 Stock Removal in Turning (G71) ........................................................................... 38

4.2.2 Stock Removal in Facing (G72) ............................................................................. 53

4.2.3 Pattern Repeating (G73) ......................................................................................... 57

4.2.4 Finishing Cycle (G70) ............................................................................................ 60

4.2.5 End F ace Peck Drilling Cycle (G74) ...................................................................... 64

4.2.6 Outer Diameter / In t ernal Diameter Drilling Cycle (G75) ..................................... 66

4.2.7 Multiple Threading Cycle (G76) ............................................................................ 68

4.2.8 Restrictio ns on Multiple Repetitive Canned Cycle (G70-G76) .............................. 74

4.2.9 Reducing path for Multiple repetitive canned cycle ............................................... 76

4.3 CANNED CYCLE FOR DRILLING ............................................................... 77

4.3.1 Front Drilling Cycle (G83)/Side Drilling Cycle (G87) .......................................... 81

4.3.2 Front Tapping Cycle (G84) / Side Tapping Cycle (G88) ....................................... 85

4.3.3 Front Boring Cycle (G85) / Side Boring Cycle (G89) ........................................... 86

c-1

Page 14

TABLE OF CONTENTS B-64694EN-1/01

4.3.4 Canned Cycle for Drilling Cancel (G80) ................................................................ 87

4.3.5 Canned Cycle for Drilling with M Code Output Improved.................................... 87

4.3.6 Reducing of Waiting Time of Spindle Speed Arrival in the

Canned Cycle for Drilling ...................................................................................... 88

4.3.7 Precautions for Operators ....................................................................................... 90

4.4 CANNED CYCLE OVERLAP FOR DRILLING ............................................. 91

4.5 RIGID TAPPING .......................................................................................... 99

4.5.1 Front Face Rigid Tapping Cycle (G84) / Side Face Rigid Tapping Cycle (G88) 100

4.5.2 Peck Rigid Tapping Cycle (G84 or G88) ............................................................. 106

4.5.3 Canned Cycle Cancel (G80) ................................................................................. 110

4.5.4 Override during Rigid Tapping ............................................................................ 111

4.5.4.1 Extraction override .......................................................................................... 111

4.5.4.2 Override signal ................................................................................................ 112

4.6 CANNED GRINDING CYCLE (FOR GRINDING MACHINE) ..................... 113

4.6.1 Traverse Grinding Cycle (G71) ............................................................................ 115

4.6.2 Traverse Direct Constant-Size Grinding Cycle (G72) ......................................... 117

4.6.3 Oscillation Grinding Cycle (G73) ........................................................................ 119

4.6.4 Oscillation Direct Constant-Size Grinding Cycle (G74) ...................................... 121

4.7 CHAMFERING AND CORNER R .............................................................. 123

4.8 MIRROR IMAGE FOR DOUBLE TURRET (G68, G69 ) ............................. 128

4.9 DIRECT DRAWING DIMENSION PROGRAMMING ................................. 130

5 COMPENSATION FUNCTION ............................................................ 135

5.1 TOOL OFFSET .......................................................................................... 135

5.1.1 Tool Geometry Offset and Tool Wear Offset ....................................................... 135

5.1.2 T Code for Tool Offset ......................................................................................... 136

5.1.3 Tool Selection....................................................................................................... 136

5.1.4 Offset Number ...................................................................................................... 136

5.1.5 Offset .................................................................................................................... 137

5.1.6 Y Axis Offset ........................................................................................................ 140

5.1.6.1 Support of arbitrary axes for Y axis offset ...................................................... 140

5.1.7 Second Geometry Tool Offset .............................................................................. 140

5.1.8 4th/5th Axis Offset ............................................................................................... 143

5.2 OVERVIEW OF TOOL NOSE RADIUS COMPENSATION (G40-G42) ..... 145

5.2.1 Imaginary Tool Nose ............................................................................................ 146

5.2.2 Direction of Imaginary Tool Nose ....................................................................... 148

5.2.3 Offset Number and Offset Value .......................................................................... 149

5.2.4 Workpiece Position and Move Command ............................................................

5.2.5 Notes on Tool Nose Radius Compensation .......................................................... 155

5.3 OVERVIEW OF CUTTER COMPENSATION (G40-G42) .......................... 158

5.4 DETAILS OF CUTTER OR TOOL NOSE RADIUS COMPENSATION ...... 163

5.4.1 Overview .............................................................................................................. 163

5.4.2 Tool Movement in Start-up .................................................................................. 167

5.4.3 Tool Movement in Offset Mode ........................................................................... 172

5.4.4 Tool Movement in Offset Mode Cancel ............................................................... 190

5.4.5 Prevention of Overcutting Due to Cutter or Tool Nose Radius Compensation ... 197

5.4.6 Interference Check ............................................................................................... 200

5.4.6.1 Operation to be performed if an interference is judged to occur ..................... 203

5.4.6.2 Interference check alarm function ................................................................... 204

5.4.6.3 Interference check avoidance function ............................................................ 205

5.4.7 Cutter or Tool Nose Radius Compensation for Input from MDI ......................... 210

5.5 VECTOR RETENTION (G38) .................................................................... 211

5.6 CORNER CIRCULAR INTERPOLATION (G39) ........................................ 212

150

c-2

Page 15

B-64694EN-1/01 TABLE OF CONTENTS

5.7 EXTENDED TOOL SELECTION ............................................................... 214

5.8 AUTOMATIC TOOL OFFSET (G36, G37) ................................................. 217

5.9 COORDINATE SYSTEM ROTATION (G68.1, G69.1) ............................... 221

6 MEMORY OPERATION USING Series 15 FORMAT ......................... 226

6.1 ADDRESSES AND SPECIFIED RANGE FOR Series 15 PROGRAM

FORMAT ................................................................................................... 226

6.2 SUBPROGRAM CALLING ........................................................................ 227

6.3 CANNED CYCLE ....................................................................................... 227

6.3.1 Outer Diameter/Internal Diameter Cutting Cycle (G90) ...................................... 228

6.3.1.1 Straight cutting cycle ....................................................................................... 228

6.3.1.2 Taper cutting cycle .......................................................................................... 229

6.3.2 Threading Cycle (G92) ......................................................................................... 230

6.3.2.1 Straight threading cycle ................................................................................... 230

6.3.2.2 Taper threading cycle ...................................................................................... 233

6.3.3 End Face Turning Cycle (G94) ............................................................................ 236

6.3.3.1 Face cutting cycle ............................................................................................ 236

6.3.3.2 Taper cutting cycle .......................................................................................... 237

6.3.4 How to Use Canned Cycles .................................................................................. 239

6.3.5 Canned Cycle and Tool Nose Radius Compensation ........................................... 240

6.3.6 Restrictio ns on Canned Cycles ............................................................................. 241

6.4 MULTIPLE REPETITIVE CANNED CYCLE .............................................. 243

6.4.1 Stock Removal in Turning (G71) ......................................................................... 244

6.4.2 Stock Removal in Facing (G72) ........................................................................... 254

6.4.3 Pattern Repeating (G73) ....................................................................................... 258

6.4.4 Finishing Cycle (G70) .......................................................................................... 260

6.4.5 End F ace Peck Drilling Cycle (G74) .................................................................... 264

6.4.6 Outer Diameter / In t ernal Diameter Drilling Cycle (G75) ................................... 266

6.4.7 Multiple Threading Cycle (G76 <G code system A/B>)

(G78 <G code system C>) .................................................................................... 268

6.4.8 Restrictions on Multiple Repetitive Canned Cycle .............................................. 274

6.5 CANNED CYCLE FOR DRILLING ............................................................. 275

6.5.1 High-speed Peck Drilling Cycle (G83.1) ............................................................. 280

6.5.2 Drilling Cycle, Spot Drilling Cycle (G81) ........................................................... 281

6.5.3 Drilling Cycle, Counter Boring (G82) ................................................................. 282

6.5.4 Peck Drilling Cycle (G83) .................................................................................... 283

6.5.5 Tapping Cycle (G84) ............................................................................................ 285

6.5.6 Boring Cycle (G85) .............................................................................................. 286

6.5.7 Boring Cycle (G89) ................................................................

6.5.8 Canned Cycle for Drilling Cancel (G80) .............................................................. 288

6.5.9 Precautions to be Taken by Operator ................................................................... 288

6.6 Canned Cycle Overlap for Drilling .............................................................. 289

.............................. 287

7 MUITI-PATH CONTROL FUNCTION .................................................. 294

7.1 BALANCE CUT (G68, G69) ....................................................................... 294

III. OPERATION

1 DATA INPUT/OUTPUT ....................................................................... 299

1.1 INPUT/OUTPUT ON EACH SCREEN ....................................................... 299

1.1.1 Inputting and Outputting Y-axis Offset Data ....................................................... 299

1.1.1.1 Inputting Y-axis offset data ............................................................................. 299

1.1.1.2 Outputting Y-axis offset data ........................................................................... 300

c-3

Page 16

TABLE OF CONTENTS B-64694EN-1/01

1.1.2 Inputting and Outputting Tool Offset / 2nd Geometry Data ................................ 301

1.1.2.1 Inputting tool offset / 2nd geometry data ......................................................... 301

1.1.2.2 Outputting tool offset / 2nd geometry data ...................................................... 302

1.1.3 Inputting and Outputting 4th/5th Axis Offset Data .............................................. 303

1.1.3.1 Inputting 4th/5th axis offset data ..................................................................... 303

1.1.3.2 Outputting 4th/5th axis offset data .................................................................. 304

1.2 INPUT/OUTPUT ON THE ALL IO SCREEN .............................................. 307

1.2.1 Inputting and Outputting Y-axis Offset Data ....................................................... 307

1.2.2 Inputting and Outputting Tool Offset / 2nd Geometry Tool Offset ..................... 309

2 SETTING AND DISPLAYING DATA ................................................... 311

2.1 SCREENS DISPLAYED BY FUNCTION KEY

2.1.1 Setting and Displaying the Tool Offset Value ..................................................... 311

2.1.2 Direct Input of Tool Offset Value Measured........................................................ 315

2.1.3 Direct Input of Tool Offset Value Measured B .................................................... 318

2.1.4 Counter Input of Offset value ............................................................................... 320

2.1.5 Setting the Workpiece Coordinate System Shift Value ........................................ 321

2.1.6 Setting Tool Offset/Second Geometry Tool Offset Values .................................. 325

2.1.7 Setting the Y-Axis Offset ..................................................................................... 328

2.1.8 Setting the 4th/5th Axis Offset ............................................................................. 334

2.1.9 Chuck and Tail Stock Barriers ............................................................................. 339

................................... 311

APPENDIX

A LIST OF FUNCTIONS INCLUDE ADDRESS P IN THE PROGRAM

COMMAND .......................................................................................... 351

A.1 LIST OF FUNCTIONS INCLUDE ADDRESS P IN THE ARGUMENT

OF G CODE .............................................................................................. 351

A.2 LIST OF FUNCTIONS INCLUDE ADDRESS P IN THE ARGUMENT

OF M AND S CODE .................................................................................. 354

c-4

Page 17

I. GENERAL

Page 18

Page 19

B-64694EN-1/01 GENERAL 1. GENERAL

NOTE

machine tool builder.

Model name

Abbreviation

NOTE

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

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

2 Some functions described in this manual may not be applied to some products. For details, refer to the DESCRIPTIONS (B-64692EN).

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 progr am 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 Describes supplementary materials.

1 This manual describes the functions that can operate in the lathe system path

control type. For other functions not specific to the lathe system, r efer to the OPERATOR'S MANUAL (Common to Lathe System/Machining Center System) (B-64694EN).

2 Some functions described in this manual may not be applied to some products.

For detail, refer to the DESCRIPTIONS manual (B-64692EN).

3 This manual does not detail the parameters not mentioned in the text. For details

of those parameters, refer to the PARAMETER MANUAL (B-64700EN).

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 t ool easily.

4 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

Applicable models

This manual describes the following models that are 'Nano CNC'. 'Nano CNC system' which realizes high precision machining can be constructed by combining these models and high speed, high precision servo controls. In the text, the abbreviations indicated below may be used.

FANUC Series 0i-TF Plus 0i-TF Plus Series 0i-F Plus Series 0i

the CNC model :

- 3 -

Page 20

1. GENERAL GENERAL B-64694EN-1/01

Manual name

Specification number

DESCRIPTIONS

B-64692EN

CONNECTION MANUAL (HARDWARE)

B-64693EN

CONNECTION MANUAL (FUNCTION)

B-64693EN-1

OPERATOR’S MANUAL (Common to Lathe System/Machining Center System)

B-64694EN

OPERATOR’S MANUAL (For Lathe System)

B-64694EN-1

OPERATOR’S MANUAL (For Machining Center System)

B-64694EN-2

MAINTENANCE MANUAL

B-64695EN

PARAMETER MANUAL

B-64700EN

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

FL-net Board CONNECTION MANUAL

B-64163EN

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

B-63874EN-2

MANUAL GUIDE i (Set-up Guidance Functions) OPERATOR’S MANUAL

B-63874EN-1

MANUAL GUIDE 0i OPERATOR’S MANUAL

B-64434EN

Dual Check Safety

Dual Check Safety CONNECTION MANUAL

B-64483EN-2

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-F Plus

The following Table 1(a) lists the manuals related to Series 0i-F Plus. This manual is indicated by an asterisk(*).

Table 1 (a) Related manuals of Series 0i-F Plus

- 4 -

B-63874EN

Page 21

B-64694EN-1/01 GENERAL 1. GENERAL

Manual name

Specification number

FANUC AC SERVO MOTOR αi series DESCRIPTIONS

FANUC AC SPINDLE MOTOR αi-B / βi-B series DESCRIPTIONS

B-65452EN

FANUC AC SERVO MOTOR βi series DESCRIPTIONS

FANUC SERVO AMPLIFIER αi-B series DESCRIPTIONS

B-65412EN

FANUC SERVO AMPLIFIER βi-B series DESCRIPTIONS

B-65422EN

FANUC AC SERVO MOTOR αi series

MAINTENANCE MANUAL

FANUC AC SERVO MOTOR αi series

PARAMETER MANUAL

Related manuals of SERVO MOTOR αi/βi series

The following Table 1(b) lists the manuals related to SERVO MOTOR αi/βi series

Table 1 (b) Related manuals of SERVO MOTOR αi/βi series

FANUC AC SERVO MOTOR αi-B series

FANUC AC SERVO MOTOR βi-B series

FANUC AC SPINDLE MOTOR αi series FANUC SERVO AMPLIFIER αi series

FANUC AC SERVO MOTOR βi series FANUC AC SPINDLE MOTOR βi series FANUC SERVO AMPLIFIER βi series

FANUC AC SERVO MOTOR βi series FANUC LINEAR MOTOR LiS series FANUC SYNCHRONOUS BUILT-IN SERVO MOTOR DiS series

FANUC AC SPINDLE MOTOR αi/βi series, BUILT-IN SPINDLE MOTOR Bi series

B-65262EN

B-65302EN

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. 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.

- 5 -

Page 22

1. GENERAL GENERAL B-64694EN-1/01

CAUTION

attempted.

CAUTION

non-volatile memory at registration, modification, or deletion of program s.

1.1 NOTES ON READING THIS MANUAL

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

1.2 NOTES ON VARIOUS KINDS OF DATA

Machining programs, parameters, offset data, etc. ar e s t ored 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. 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 t he

- 6 -

Page 23

II. PROGRAMMING

Page 24

Page 25

B-64694EN-1/01 PROGRAMMING 1. GENERAL

Workpiece

Standard tool

Rough cutting tool

Finishing tool

Grooving tool

Threading tool

1 GENERAL

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 differ ence 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. (Refer to the section of Section 5.1 “TOOL OFFSET”.)

Fig. 1.1 Tool offset

- 9 -

Page 26

PROGRAMMING B-64694EN-1/01

2. PREPARATORY FUNCTION (G FUNCTION)

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_ ; :

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.

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 u se 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. 340 2) 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 wit h (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) When G code system B or C is used, setting bit 3 (G91) of parameter No. 3402 determines

which code, either G90 or G91, is effectiv e.

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 ar e specified in th e same block, only the last G cod e 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 incr emental 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 2(a).

- 10 -

Page 27

B-64694EN-1/01 PROGRAMMING

2. PREPARATORY FUNCTION

Table 2(a) G code list

G code system

A B C

G00

Positioning (Rapid traverse)

G01

Linear interpolation (Cutting feed)

G02

Circular interpolation CW or helical interpolation CW

G03

Circular interpolation CCW or helical interpolation CCW

G04

Dwell

G04.1

G code preventing buffering

contour control)

G05.1

AI contour control

G05.4

HRV3 on/off

(G107)

command)

G09

Exact stop

G10

Programmable data input

G10.6

Tool retract and recover

G11

Programmable data input mode cancel

(G112)

(G113)

G17

XpYp plane selection

G18

ZpXp plane selection

G19

YpZp plane selection

G20

G70

Input in inch

G21

G71

Input in mm

G22

Stored stroke check function on

G23

Stored stroke check function off

G25

Spindle speed fluctuation detection off

G26

Spindle speed fluctuation detection on

G27

Reference position return check

G28

Return to reference position

G28.2

In-position check disable reference position return

G29

Movement from reference position

G30

2nd, 3rd and 4th reference position return

return

G31

Skip function

G31.8

EGB-axis skip

G32

G33

Threading

G34

Variable lead threading

G35

Circular threading CW

(G36) of parameter No. 3405 is set to 0)

No. 3405 is set to 0)

No. 3405 is set to 1)

Group Function

(G FUNCTION)

G05 G05 G05

G07.1

G08 G08 G08

G12.1

G13.1

G07.1

G12.1

G13.1

G07.1

G12.1

G13.1

AI contour control (command compatible with high precision

Cylindrical interpolation AI contour control (advanced preview control compatible

Polar coordinate interpolation mode

Polar coordinate interpolation cancel mode

G30.2 G30.2 G30.2

G36 G36 G36

G37 G37 G37

G37.1 G37.1 G37.1

G37.2 G37.2 G37.2

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

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

Automatic tool offset (Z axis) (When bit 3 (G36) of parameter

Automatic tool offset (X axis) (When bit 3 (G36) of parameter

Automatic tool offset (Z axis) (When bit 3 (G36) of parameter

- 11 -

Page 28

PROGRAMMING B-64694EN-1/01

2. PREPARATORY FUNCTION (G FUNCTION)

Table 2(a) G code list

G code system

A B C

G38

Tool radius/tool nose radius compensation: with vector held

interpolation

G40

Tool radius/tool nose radius compensation : cancel

G41

Tool radius/tool nose radius compensation : left

G42

Tool radius/tool nose radius compensation : right

G40.1

Normal direction control cancel mode

G41.1

Normal direction control left on

G42 .1

Normal direction control right on

(G44.7)

(Bit 3 (TCT) of parameter No. 5040 mus t be "1".)

G50

G92

Coordinate system setting or max spindle speed clamp

G50.3

G92.1

Workpiece coordinate system preset

G50.1

Programmable mirror image cancel

G51.1

Programmable mirror image

G50.2

(G250)

G50.2

(G250)

G50.2

(G250)

(G251)

G50.4

Cancel synchronous control

G50.5

Cancel composite control

G50.6

Cancel superimposed control

G51.4

Start synchronous control

G51.5

Start composite control

G51.6

Start superimposed control

G52

Local coordinate system setting

G53

Machine coordinate system setting

G53.1

Tool axis direction control

G53.2

Selecting a machine coordinate system with feedrate

G53.6

Tool center point retention type tool axis direction contr ol

(G54.1)

G55

Workpiece coordinate system 2 selection

G56

Workpiece coordinate system 3 selection

G57

Workpiece coordinate system 4 selection

G58

Workpiece coordinate system 5 selection

G59

Workpiece coordinate system 6 selection

G61

Exact stop mode

G63

Tapping mode

G64

Cutting mode

G65

Macro call

G66

Macro modal call A

G66.1

Macro modal call B

G67

Macro modal call A/B cancel

G68

Mirror image on for double turret or balance cutting mode

system conversion mode on

G68.2

Tilted working plane indexing command

G68.3

Tilted working plane indexing command by tool axis direction

multi-command)

Group Function

G39 G39 G39

G43.7

G51.2

G43.7

G51.2

G43.7

G51.2

Tool radius/tool nose radius compensation: corner roundi ng

Tool offset

Polygon turning cancel

Polygon turning

G54

G68.1 G68.1 G68.1

G54

Workpiece coordinate system 1 selection

Coordinate system rotation start or 3-dimensional coordinate

G68.4 G68.4 G68.4

Tilted working plane indexing command (incremental

- 12 -

Page 29

B-64694EN-1/01 PROGRAMMING

2. PREPARATORY FUNCTION

Table 2(a) G code list

G code system

A B C

coordinate system conversion mode off

G70

G72

Finishing cycle

G71

G73

Stock removal in turning

G72

G74

Stock removal in facing

G73

G75

Pattern repeating cycle

G74

G76

End face peck drilling cycle

G75

G77

Outer diameter/internal diameter drilling cycle

G76

G78

Multiple-thread cutting cycle

G71

G72

Traverse grinding cycle

G72

G73

Traverse direct sizing/grinding cycle

G73

G74

Oscillation grinding cycle

G74

G75

Oscillation direct sizing/grinding cycle

Electronic gear box : synchronization cancellation

G81.1

High precision oscillation function

G80.4

Electronic gear box: synchronization cancellation

G81.4

Electronic gear box: synchronization start

G80.5

Electronic gear box 2 pair: synchronization cancellation

G81.5

Electronic gear box 2 pair: synchronization start

Electronic gear box : synchronization start

G82

Counter boring (FS15-T format)

G83

Cycle for face drilling

G83.1

High-speed peck drilling cycle (FS15-T format)

G83.5

High-speed peck drilling cycle

G83.6

Peck drilling cycle

G84

Cycle for face tapping

G84.2

Rigid tapping cycle (FS15-T format)

G85

Cycle for face boring

G87

Cycle for side drilling

G87.5

High-speed peck drilling cycle

G87.6

Peck drilling cycle

G88

Cycle for side tapping

G89

Cycle for side boring

G90

G77

G20

Outer diameter/internal diameter cutting cycle

G92

G78

G21

Threading cycle

G94

G79

G24

End face turning cycle

G91.1

Maximum specified incremental amount check

G96

Constant surface speed control

G97

Constant surface speed control cancel

G96.1

Spindle indexing execution (waiting for completion)

G96.2

Spindle indexing execution (not waiting for completion)

G96.3

Spindle indexing completion check

G96.4

SV speed control mode ON

G98

G94

Feed per minute

G99

G95

Feed per revolution

Group Function

G69 G69 G69

Mirror image off for double turret or balance cutt ing mode cancel

(G FUNCTION)

G69.1 G69.1 G69.1 17

G80 G80

G81 G81 G81

G80

Coordinate system rotation cancel or 3-dimensional

Canned cycle cancel for drilling

Spot drilling (FS15-T format)

- 13 -

Page 30

PROGRAMMING B-64694EN-1/01

2. PREPARATORY FUNCTION (G FUNCTION)

Table 2(a) G code list

G code system

A B C

G90

Absolute programming

G91

Incremental programming

G98

Canned cycle : return to initial level

G99

Canned cycle : return to R point level

Group Function

- 14 -

Page 31

B-64694EN-1/01 PROGRAMMING 3. INTERPOLATION FUNCTION

Straight thread

Tapered

screw

Scroll thread

X axis

Start point

End point_

Z axis

G32IP_F_; IP_: End point

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

3 INTERPOLATION FUNCTION

3.1 THREADING (G32)

Tapered screws and scroll threads in addition to equal lead straight th reads 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

Fig. 3.1 (a) Thread types

Fig. 3.1 (b) Example of threading

- 15 -

Page 32

3. INTERPOLATION FUNCTION PROGRAMMING B-64694EN-1/01

Tapered thread

a≤45° lead is LZ a≥45° lead is LX

Least command increment

Metric input

0.0001 to 500.0000 mm

Inch input

0.000001 to 9.999999 inch

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.

Fig. 3.1 (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 3.1 (a) lists the ranges for specifyin g the thread lead.

Table 3.1 (a) Ranges of lead sizes th at can be specified

- Continuous threading

The "continuous threading" is effective for G32.

Limitation

- Tool Retract and Recover

When the major axis for threading is specified as th e retraction axis, retraction is not performed. In this case, after a block that does not specify threading is executed, an alarm PS0429, “ILLEGAL COMMAND IN G10.6” is issued and the tool sto ps.

- Chamfering and Corner R

Chamfering or corner R cannot be specified in a block in which thread cutting is specified. If tool offset is specified, alarm PS0050, “CHF/CNR NOT ALLOWED IN THRD BLK”, is issued.

- Tool offset

Tool offset cannot be specified in a block in which thread cutting is specified. If tool offset is specified, alarm PS0509, “TOOL OFFSET COMMAND IS NOT AVAILABLE”, i s issued.

- 16 -

Page 33

B-64694EN-1/01 PROGRAMMING 3. INTERPOLATION FUNCTION

Z axis

X axis

The following values are used in programming : Thread lead :4mm δ1=3mm δ2=1.5mm 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 ;

1. Straight threading

Z axis

X axis

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

=2mm δ2=1mm 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 ;

f50

f43

f14

2.Tapered threading

CAUTION

1 Feedrate override is effective (fixed at 100%) during threading.

execution of the first block not specifying threading.

Example

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, Feed hold lamp signal SPL turns to “1” immediately after feed hold signal *SP is set to “1”. Then, when the tool stops, the signal SPL turns to “0” (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

- 17 -

Page 34

3. INTERPOLATION FUNCTION PROGRAMMING B-64694EN-1/01

CAUTION

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

MANUAL (Common to Lathe System/Machining Center System) (B-64694EN).

G32

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 contr ol dur ing 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 funct ion is inef f ec t ive to G32. 12 If tool offset (with t he T c ode or G43.7) is specified in during of the threading

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

IS NOT AVAILABLE”, is issued. 13 The leads of a thread are generally incorrect , due to automatic acceleration and

deceleration. Thus distance allowances must be made to the extent in the

program. Refer “INCORRECT THREADED LENGTH” in the OPERATOR’S

3.2 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 th at the synchro nism 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.

Fig. 3.2 (a) Continuous threading (Example of G32 in G code system A)

Even when the same section is repeated for threadin g while changing the depth of cu t, this sy stem allows a correct machining without impairing the threads.

- 18 -

Page 35

B-64694EN-1/01 PROGRAMMING 3. INTERPOLATION FUNCTION

L : Lead

(Threading)

(Increment: 0.001 degrees, Valid setting range: 0 to 360 degrees)

- Available threading commands

G32: Threading (G code system A) G33: 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.

3.3 MULTIPLE THREADING

Using the Q address to specify an angle b etween 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.

Format

Explanation

- Available threading commands

Limitation

- Threading start angle

Fig. 3.3 (a) Multiple thread screws.

G32 IP _ F_ Q_ ;

IP : End point F_ : Lead in longitudinal direction

G32 IP _ Q_ ;

Q_ : Angle for shifting the threading start angle

G32: Threading G34: Variable lead threading G35, G36: Circular threading G76/G78: Multiple threading cycle (Only when the FS15 tape format is used.) G92: Threading cycle

The threading 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.

- 19 -

Page 36

3. INTERPOLATION FUNCTION PROGRAMMING B-64694EN-1/01

Program for producing double-threaded screws (w i th threading start angles of 0

Cutting start point of 2nd

Cutting start point of 1st

180°

Z axis

δ δ

Thread lead :4mm

Threading start angle of 2nd :180 degree

- Threading start angle increment

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

The threading 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 Q9000 0 (90 degrees).

- Direction of start angle

The direction of start angle is changed by the direction of spindle rotation because it is delayed from one-spindle- rotation signal.

- 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 FS15 tape format is used, in G76 /G78 multiple thread ing cycle, th e address Q is possi ble to specify the angle for shifting the threading start angle.

Example

and 180 degrees)

G00 X40.0 ; G32 W-38.0 F4.0 Q0 ; G00 X72.0 ; W38.0 ; X40.0 ; G32 W-38.0 F4.0 Q180000 ; G00 X72.0 ; W38.0 ;

δ1=5mm δ2=3mm Depth of cut :1mm (Metric input, diameter programming)

Threading start angle of 1st :0 degree

- 20 -

Page 37

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

NOTE

XY plane: Y-axis direction

4 FUNCTIONS TO SIMPLIFY PROGRAMMING

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).

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

- 21 -

Page 38

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

G90X(U)_Z(W)_F_;

F_ : Cutting feedrate

X/2

X axis

Z axis

2(F)

3(F)

1(R)

4(R)

U/2

A’

(R)....Rapid traverse

(F)....

Cutting feed

NOTE

cycle start button once.

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

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

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).)

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

- Canceling the mode

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

Fig. 4.1.1.1 (a) Straight cutting cycle

- 22 -

Page 39

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

G90 X(U)_Z(W)_R_F_;

F_ : Cutting feedrate

3(F)

X/2

4(R)

U/2

1(R)

Z axis

2(F) R

X axis

A’

(R)....

Rapid traverse

(F) ....

Cutting feed

NOTE

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

NOTE

cycle start button once.

4.1.1.2 Taper cutting cycle

Format

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))

Fig. 4.1.1.2 (a) Taper cutting cycle

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.

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

- 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.

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

- 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).

- 23 -

Page 40

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Outer diameter machining

Internal diameter machining

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

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

U/2

3(F)

4(R)

1(R)

2(F)

U/2

3(F)

4(R)

1(R)

2(F)

at |R|≤|U/2|

U/2

3(F)

4(R)

1(R)

2(F)

U/2

3(F)

4(R)

1(R)

2(F)

G92 X(U)_Z(W)_F_Q_;

F_ : Thread lead (L in the Fig. 4.1.2.1 (a))

Table 4.1.1.2 (a)

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

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

- Canceling the mode

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

4.1.2 Threading Cycle (G92)

4.1.2.1 Straight threading cycle

Format

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)

- 24 -

Page 41

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

X/2

X axis

Z axis

1(R)

2(F)

3(R)

4(R)

Detailed chamfered thread

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

Approx.

45°

(R) ...Rapid traverse

(F).... Cutting feed

A’

U/2

CAUTION

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

NOTE

cycle start button once.

Fig. 4.1.2.1 (a) Straight threading

Explanation

The ranges of thread leads and restrictions related to the spind le speed are the same as for threading wit h 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 Z X 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 plan e (start Z-coordinate for

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

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

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

- Canceling the mode

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

- Accelerat ion/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.

- 25 -

Page 42

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

NOTE

are used for this cycle and threading cycle with G76.

Bit 0 (CFR) of

parameter No. 1611

Parameter No.

1466

No. 1627), and retraction feedrate specified in parameter No. 1466.

No. 1627), and rapid traverse rate specified in parameter No. 1420.

(parameter No. 1420).

NOTE

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

- Time constant and FL feedrate for threading

The time constant for acceleration/deceleration after interpol ation fo r thread ing sp ecified i n 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 chamf er ing

Thread chamfering can be performed. A signal from the machine tool, ini tiates 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.

Common parameters for specifying the amount and angle of thread chamfer ing

- Retract ion 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)

Description

Uses the type of acceleration/deceleration after interpolat i on for threading,

0 Other than 0

0 0

time constant for threading (parameter No. 1626), FL feedrate (parameter

Uses the type of acceleration/deceleration after interpolat i on for threading, time constant for threading (parameter No. 1626), FL feedrate (parameter

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

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

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

- 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.

- Feed hold i n a t hr eading cycle

When the Threading cycle retract function is invalid, the behavior of feed hold is as follows:

- If bit 3 (TFH) of parameter No.5109 is 0 and FEED HOLD button is pressed and released in the

threading, the tool returns to end point of operation 4 and stops. If FEED HOLD is kept pressed, the tool stops at the vicinity of the end point of retraction (end point of operation 3).

- 26 -

Page 43

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Feed hold is effected here.

Start point Ordinary cycle

Rapid traverse

Motion at feed hold

X axis

Z axis

Cutting feed

CAUTION

Another feed hold cannot be made during retreat.

G92 X(U)_Z(W)_R_F_Q_;

F_ : Thread lead (L in the Fig. 4.1.2.2 (a))

- If bit 3 (TFH) of parameter No.5109 is 1 and FEED HOLD button is pressed and released or kept

pressed in the threading, the tool stops at the end point of retraction (end point of operation 3).

- Threading cycle retract

When the Threading cycle retract function is enabled, feed hold may be applied during threading (operation 2). In this case, the tool immediately retracts with chamfering an d returns to th e start point on the second axis (X-axis), then the first axis (Z-axis) on the plane.

Fig. 4.1.2.1(b)

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

- Inch t hr eadi ng

Inch threading specified with address E is not allowed.

4.1.2.2 Taper threading cycle

Format

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))

- 27 -

Page 44

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Detailed chamfered thread

1(R)

Z axis 3(R)

4(R)

2(F)

U/2

X/2

X axis

Approx. 45°

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

(R)....

Rapid traverse

(F) ....

Cutting feed

A’

NOTE

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

CAUTION

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

Fig. 4.1.2.2 (a) Taper threading cycle

Explanation

The ranges of thread leads and restrictions related to the spind le 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.

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

- 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.

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

- 28 -

Page 45

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

NOTE

cycle start button once.

Outer diameter machining

Internal diameter machining

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

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

U/2

3(F)

4(R)

1(R)

2(F)

U/2

3(F)

4(R)

1(R)

2(F)

at |R|≤|U/2|

U/2

3(F)

4(R)

1(R)

2(F)

U/2

3(F)

4(R)

1(R)

2(F)

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

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

Table 4.1.2.2 (a)

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

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

- Canceling the mode

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

- Accelerat ion/deceleration after interpolation for threading

- Time constant and FL feedrate for threading

- Thread chamf er ing

- Retract ion after chamfering

- Feed hold i n a t hr eading cycle

- Shifting the start angle

- Threading cycle retract

- Inch t hr eadi ng

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

- 29 -

Page 46

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

G94 X(U)_Z(W)_F_;

F_ : Cutting feedrate

X axis

4(R)

X/2 3(F)

Z axis 1(R)

2(F) Z

(R)... Rapid traverse

(F).... Cutting feed

U/2

A’

NOTE

cycle start button once.

4.1.3 End Face Turning Cycle (G94)

4.1.3.1 Face cutting cycle

Format

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

Fig. 4.1.3.1 (a) Face cutting cycle

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).)

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

- Canceling the mode

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

- 30 -

Page 47

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

G94 X(U)_Z(W)_R_F_;

F_ : Cutting feedrate

(R) .... Rapid traverse

(F) .... Cutting feed

4(R)

X/2 3(F)

Z axis

1(R)

2(F)

U/2

X axis

A’

NOTE

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

NOTE

cycle start button once.

4.1.3.2 Taper cutting cycle

Format

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))

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.

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

- 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 plan e (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.

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

Fig. 4.1.3.2 (a) Taper cutting cycle

- 31 -

Page 48

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Outer diameter machining

Internal diameter machining

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

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

1(R)

U/2

3(F)

4(R)

2(F)

U/2

3(F)

4(R)

2(F)

1(R)

3. U < 0, W < 0, R > 0 at |R|≤|W|

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

at |R|≤|W|

U/2

3(F)

4(R)

2(F)

1(R)

Z X

U/2

3(F)

4(R)

2(F)

1(R)

Shape of product

Shape of material

- 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)

- 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)

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

- Strai ght cutting cycle (G90)

- 32 -

Page 49

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Shape of product

Shape of material

Shape of product

Shape of material

Shape of product

Shape of material

- Taper cutting cycle (G90)

- Face cutt i ng cycle (G94)

- Face taper cutting cycle (G94)

- 33 -

Page 50

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

Tool nose radius center path

Offset direction

Total tool nose

Tool nose radius center path

Programmed path

845

Total tool nose

Tool nose radius center path

Programmed path

Total tool nose

Tool nose radius center path

Offset direction

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 cycl e, 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)

End face cutting cycle (G94)

Threading cycle (G92)

Tool nose radius compensation cannot be applied.

- 34 -

Page 51

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

NOTE

refer to "FANUC Series 16i/18i/21i OPERATOR'S MANUAL."

G90 G94

4,8,3

5,0,7

1,6,2

4,5,1

8,0,6

3,7,2

Total tool nose

Tool nose radius center path

Programmed path

4,5,1

8,0,6

3,7,2

Total tool nose

4,8,3

5,0,7

1,6,2

Programmed path

Tool nose radius center path

Differences between this CNC and the FANUC Series 16i/18i/21i

This CNC is the same as the FANUC Series 16i/18i/21i 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 16i/18i/21i 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,

How compensation is applied for the FANUC Series 16i/18i/21i

4.1.6 Restrictions on Canned Cycles

Limitation

- Modal

Since data items X (U), Z (W), and R in a canned cycle are modal valu es common to G90 , G92, and G9 4. 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.

- 35 -

Page 52

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

Example

Workpiece

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;

Example

N012 G90 X20.5 Z10.0;

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 v alues. If no modal values are specified, no cycle operatio ns are performed. When G04 is specified, G04 is executed and no canned cycle is performed.

- 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.

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

←

- Plane selection command

Specify a plane selection command (G17, G18, o r G19) before setting a canned cycle or specify it in the block in which the first canned cycl e is specified. If a plane selection command is specified in the canned cycle mode, the command is execut ed, but the modal values common to canned cycles are cleared. If an axis which is not on the selected plan e is specified, alarm PS033 0, “ILLEGAL AXIS COMMAND IS IN THE TURNING CANNED CYCLE” is issued.

- Parall el axis

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

Cancels the canned cycle mode.

- 36 -

Page 53

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

NOTE

V, and W cannot be set as a parallel axis.

1(R)

3(F)

4(R)

2(F)

Cancellation

- 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 i ntervention

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

Manual intervention

4.2 MULTIPLE REPETITIVE CANNED CYCLE (G70-G76)

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

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 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,

- 37 -

Page 54

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

ZpXp plane

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

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

YpZp plane

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

4.2.1 Stock Removal in Turning (G71)

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

Format

G71 U(∆d) R(e) ; G71 P(ns) Q(nf) U(∆u) W(∆w) F(f ) S(s ) T(t ) ;

G71 W(∆d) R(e) ; G71 P(ns) Q(nf) V(∆w) W(∆u) F(f ) S(s ) T(t ) ; N (ns) ; ... N (nf) ;

XpYp plane

G71 V(∆d) R(e) ; G71 P(ns) Q(nf) U(∆w) V(∆u) F(f ) S(s ) T(t ) ; N (ns) ; ... N (nf) ;

∆d : 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. ∆u : Distance of the finishing allowance in the direction of the second axis on the plane

(X-axis for the ZX plane) ∆w : 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

- 38 -

Page 55

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

input

system for the reference axis.

required

system for the reference axis.

required

system for the reference axis.

for the second axis on the plane.

system for the reference axis.

for the first axis on the plane.

(R)

(F)

∆u/2

∆d

A’

∆

Target figure

45°

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

e: Escaping amount

NOTE

previous block is effective.

Unit Diameter/radius programming Sign

Depends on the increment

∆d

Depends on the increment

∆u

Depends on the increment

∆w

Radius programming

Radius programming Depends on diameter/radius programming

Depends on diameter/radius programming

Decimal point

Not

Required Allowed

Allowed

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

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 ∆d (depth of cut), with the finishing allowance specified by ∆u/2 and ∆w 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.

1 While both ∆d and ∆u 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 constant surface speed control 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 G71 block or the

- 39 -

Page 56

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Both linear and circular interpolation are possible

U(+)…W(+)

U(+)…W(-)

U(-)…W(+)

U(-)…W(

NOTE

compensation is applied is checked.

- 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 ∆u and ∆w are as follows:

Fig. 4.2.1 (b) Four target figure patterns

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 fir st and second axes on

the plane.

(3) For type II, the figure must show monot one 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.

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

- 40 -

Page 57

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

Check

Related parameter

Q is contained in the program before cycle operation.

5102 is set to 1.

Checks the target figure before cycle operation.

address Q is contained.)

Enabled when bit 2 (FCK) of parameter No.

Example

N200…………;

The following checks can also be made.

Checks that a block with the sequence number specified at address

(Also checks that a block with the sequence number specified at

Enabled when bit 2 (QSR) of parameter No.

5104 is set to 1.

- 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. Wi th 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 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 plan e (X-axis for th e ZX plane) an d first axis o n the plan e (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 prog ramming 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.

ZX plane G71 U10.0 R5.0 ;

G71 P100 Q200....;

N100 X(U)_ ;

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

- 41 -

Page 58

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

No pockets are allowed.

A’

CAUTION

case.

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

45°

(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)

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 MONOTO NOUS 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

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

It can be changed escape after rough cutting to the rapid traverse by setting bit 0 (CBR) of parameter No.5124 to 1. The tool path follows the setting in bit 1 (LRP) of parameter No. 1401 during escape.

(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.

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

- 42 -

Page 59

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

(F)

∆u/2

∆d

A’

∆W

Target figure

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

(R)

∆d

(F)

(R)

Example

N200…………;

. . .

- Type II

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

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 ∆d (depth of cut), with the finishing allowance specified by ∆u/2 and ∆w 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 ∆u/2 and ∆w left.

Type II differs from type I in the following points: (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.

ZX plane G71 U10.0 R5.0;

G71 P100 Q200.......;

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

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

(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 hav e concaves (pockets).

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

- 43 -

Page 60

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Monotone change is not observed along the Z-axis.

CAUTION

in parameter No. 5145 to specify that the alarm is not issued in this case.

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

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

Escaping after cutting

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.

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

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 t he m ov em ent 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

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).

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.

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

- 44 -

Page 61

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

e (specified in the command or

parameter No. 5133)

45°

Bottom

Depth of cut ∆d



Start point



Escaping operation after rough cutting

Escaping operation after rough cutting as finishing

<1>

<2>

<3>

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

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

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 hei gh t eq uals to that at the start point, the tool passes through the point in the position obtained by adding depth of cut ∆d 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 ∆d 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.

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

(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)

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

- 45 -

Page 62

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

<3>

<2>

<1>

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

•

Rapid traverse

Escaping from the bottom

Cutting feed

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

plane)

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

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

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

The following Fig. 4.2.1(o) shows how the tool moves after rough cutting for a pocket in detail.

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

Cuts the workpiece at the cutting feedrate an d 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)

- 46 -

Page 63

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

CAUTION

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

1 This CNC differs from the FANUC Series 16i/18i/21i in cutting of a pocket. The tool first cuts the nearest pocket to the start point. Af t er cutting of the pocket

terminates, the tool moves to the nearest but one pocket and start s c ut ting.

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

This CNC differs from the FANUC Series 16i/18i/21i 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).

- Tool nose radius compensation

When using tool nose radius compensation, specify a tool nose radius compensation command (G41, G42) before a multiple repetitive canned cy cle 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, o ffset 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 p oin t 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).

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

- 47 -

Page 64

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Cycle start point

Start-up



Offset cancel

Start-up

Offset cancel

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

A’

Tool nose center path when tool nose radius compensation is applied with G42

Position between AA' in which start-up is performed

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

Tool nose center path when tool nose radi us compensation is applied with G42

A’

Position between A-A' in which startup is performed

Fig. 4.2.1 (q)

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'.

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

Fig. 4.2.1 (s)

- 48 -

Page 65

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

NOTE

pocket. This prevents a pocket from being dug.

For the type I command

: Rapid traverse can be selecte d.

: The mode specified in the start block is followed.

Operation 1

Operation 2

Previous turning point

Current turning point

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

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. (2) Command G41/G42 at the first block of the target figure program (commanded by P address) If G41 or G42 is commanded in the target figure program other than the first block, the PS0325

alarm “UNAVAILABLE COMMAND IS IN SHAPE PROGRAM” is occurred. (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 ... ;

- Reducing the cycle tim e

In G71 and G72, the tool can be moved to the previous turning start point (operation 1) in rapid traverse by setting bit 0 (ASU) of parameter No. 5107 to 1. Bit 0 (ASU) of parameter No. 5107 is valid for both type I and II commands.

Fig. 4.2.1 (t)

- 49 -

Page 66

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

For the type II command

Operation 1

Operation 2

Previous turning point

Current turning point

Cycle start point

Path of DTP = 1

Path of DTP = 0

End point of finishing

shape

Cycle start point ＋

Distance of the finishing

allowance

For the type I G71 and G72 commands, operations 1 and 2 to the current turning start point that are usually performed in 2 cycles can be performed in 1 cycle by setting bit 1 (ASC) of parameter No. 5107 to 1. The feed mode specified in the start block in the program for a target figure (G00 or G01) is used. Bit 1 (ASC) of parameter No. 5107 is valid only for the type I command.

Fig. 4.2.1 (u)

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.

Fig. 4.2.1 (v) 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.)

- 50 -

Page 67

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

A B

(1)

(2)

(3)

(4)

(1)

(2)

(3)

(4)

- 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).

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

Fig. 4.2.1 (x) 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 th e path AB is executed by rap id traverse at second times. The overlap path CD is avoided.

Fig. 4.2.1 (y) Target figure with pocket (No.5108#3=0)

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

- 51 -

Page 68

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

A B C

Rapid traverse movement Cutting movement Ignored in

-position check point

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

then performs positioning to the start point of a next pocket as shown in 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 at the first time and then the pocket cutting is executed one after another.

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

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

When bit 5 (NIC) of parameter No. 5108 is set to 1, the in-position check between cutting blocks is not executed. Therefore this has effects on the cycle time reduction. If the large value is set to parameter No. 1826/ No. 1827 as the in-position width, bit 5 (NIC) of parameter No. 5108 is not effective.

Fig. 4.2.1 (cc) Improvement of in-position check

- 52 -

Page 69

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

ZpXp plane

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

;

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

YpZp plane

or T function in this G72 block is effective.

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

G72 W(∆d) R(e) ; G72 P(ns) Q(nf) U(∆u) W(∆w) F(f ) S(s ) T(t ) ;

G72 V(∆d) R(e) ; G72 P(ns) Q(nf) V(∆w) W(∆u) F(f ) S(s ) T(t ) ; N (ns) ; ... N (nf) ;

XpYp plane

G72 U(∆d) R(e) ; G72 P(ns) Q(nf) U(∆w) V (∆u) F(f ) S(s ) T(t ) ; N (ns) ; ... N (nf) ;

∆d : 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 Thi s 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) ∆w : 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 is ignored in the cycle, and the F, S,

- 53 -

Page 70

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

input

system for the reference axis.

required

system for the reference axis.

required

system for the reference axis.

for the second axis on the plane.

system for the reference axis.

for the first axis on the plane.

∆u/2 ∆d

Tool path

(F) (R)

e 45°

(R)

(F)

∆w

Target figure

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

NOTE

previous block is effective.

Unit Diameter/radius programming Sign

Depends on the increment

∆d

Depends on the increment

∆u

Depends on the increment

∆w

Radius programming

Radius programming Depends on diameter/radius programming

Depends on diameter/radius programming

Decimal point

Not

Required Allowed

Allowed

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

Explanation

- Operations

1 While both ∆d and ∆u 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 constant surface speed control 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

- 54 -

Page 71

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Both linear and circular interpolation are possible

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

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

U(+)...

W(+)...

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

NOTE

compensation is applied is checked.

- 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 ∆u and ∆w are as follows:

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

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 fir st and second axes on

the plane.

(3) For type II, the figure must show monot one 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, either type I or II is also selected. 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.

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

The following checks can also be made.

- 55 -

Page 72

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

Check

Related parameter

Q is contained in the program before cycle operation.

No. 5102 is set to 1.

address Q is contained.)

Checks that a block with the sequence number specified at address

Checks the target figure before cycle operation. (Also checks that a block with the sequence number specified at

Enabled when bit 2 (QSR) of parameter

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

- 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. Wi th type I, the tool escapes to the direction of 45 degrees. With type II, the tool escapes from 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 plan e (X-axis for th e 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 prog ramming with travel distance 0 (U0 for the ZX plane).

- Type I

G72 differs from G71 in the following points: (1) G72 cuts the workpiece by 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 by 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 the rough cuttings along the second axis on the plane (X-axis for the ZX plane) have

terminated, 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 tim e

See the pages on which G71 is explained.

- 56 -

Page 73

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

ZpXp plane

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

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

YpZp plane

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

4.2.3 Pattern Repeating (G73)

Format

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

G73 W(∆k) U(∆i) R(d) ; G73 P(ns) Q(nf) U(∆u) W(∆w) F(f ) S(s ) T(t ) ;

G73 V(∆k) W(∆i) R(d) ; G73 P(ns) Q(nf) V(∆w) W(∆u) F(f ) S(s ) T(t ) ; N (ns) ; ... N (nf) ;

XpYp plane

G73 U(∆k) V(∆i) R(d) ; G73 P(ns) Q(nf) U(∆w) V(∆u) F(f ) S(s ) T(t ) ; N (ns) ; ... N (nf) ;

∆i : 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.

∆k : Distance of escape in the di rec ti on of the fi rst 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. ∆u : Distance of the finishing allowance in the direction of the second axis on the plane

(X-axis for the ZX plane) ∆w : 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

- 57 -

Page 74

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

input

system for the reference axis.

the second axis on the plane.

system for the reference axis.

the first axis on the plane.

NOTE

number of division.

∆w

∆u/2

∆i+∆u/2

∆k+∆w

∆w

∆u/2

Target figure

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

(R)

(F)

NOTE

S, and T functions.

Unit Diameter/radius programming Sign

Depends on the increment

∆i

Depends on the increment

∆k

Depends on the increment

∆u

Depends on the increment

∆w

Radius programming Required Allowed

Radius programming Required Allowed Depends on diameter/radius programming for

Depends on diameter/radius programming for

Required Allowed

Decimal point

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

Fig. 4.2.3 (a) Cutting path in pattern repeating

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 ∆u/2 and ∆w left.

1 While the values ∆i and ∆k, or ∆u and ∆w 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,

- 58 -

Page 75

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Check

Related parameter

Q is contained in the program before cycle operation.

No. 5102 is set to 1.

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;

N10

N15

N20

N30

- Target figure Patterns

As in the case of G71, there are four target figure pat terns. Be careful about signs of ∆u, ∆w, ∆i, and ∆k 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.

Checks that a block with the sequence number specified at address

Enabled when bit 2 (QSR) of parameter

- 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 is the end point of each cycle and the end point of each block in the finishing shape. When bit 2 (PRS) of parameter No. 5125 is set to 1, the stop position of single block operation is the end point of each cycle 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).

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

- 59 -

Page 76

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

G70 P(ns) Q(nf) ;

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

Check

Related parameter

Q is contained in the program before cycle operation.

No. 5102 is set to 1.

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 is the end point of each cycle and the end point of each block in the finishing shape as shown in Fig. 4.2.3 (d). The single block stop is not executed at the end point of escape from the cycle start poi nt. 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 is the end point of each cycle 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.

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

4.2.4 Finishing Cycle (G70)

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

Format

ns : Sequence number of the first 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 too l 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.

Checks that a block with the sequence number specified at address

Enabled when bit 2 (QSR) of parameter

- Stori ng 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 ind icated by P and Q are immediately found at execution of G70 without

- 60 -

Page 77

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

Example

cycles)

NOTE

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

NOTE

from the end point of the target figure to the cycle start point.

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 thi s time, for the fourth and subsequent rough cutting cycles, the cycle time is longer because memory is searched for P and Q blocks.

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

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

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

- Return t o 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.

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

- 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 cy cle command (G70) and specify the cancel command (G4 0) 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.

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'.

- 61 -

Page 78

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Example

- 62 -

Page 79

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

- 63 -

Page 80

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

G74R (e) ;

f : Feedrate

Diameter/radius

programming

Decimal point

input

the reference axis.

NOTE

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

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

G74X(U)_ Z(W)_ P(∆i) Q(∆k) R(∆d) 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.) ∆i : Travel distance in the direction of the second axis on the plane (X-axis for the ZX

plane)

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

Unit

Depends on the increment system for

∆i

Depends on the increment system for

∆k

Depends on the increment system for

∆d

Radius programming Not required Allowed

Radius programming Not required Not allowed

Radius programming NOTE Allowed

Sign

Normally, specify a positive value for ∆d. When X (U) and ∆i are omitted, specify

- 64 -

Page 81

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

U/2

∆d

∆i’

∆k'

∆k

(R)

(F)

(R)

(F)

∆i

[0 < ∆k’

≤ ∆k]

(R)

[0 < ∆i’ ≤ ∆i]

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

NOTE

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

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

Explanation

- Operations

A cycle operation of cutting by ∆k and return by e is repeated. When cutting reaches point C, the too l escapes by ∆d. Then, the tool returns in rapid traverse, moves to the direction of point B by ∆i, and performs cutting again.

1 While both e and ∆d 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, ∆d is used.

- Tool nose radius compensation

Tool nose radius compensation cannot be applied.

- 65 -

Page 82

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

G75R (e) ;

f : Feedrate

input

the reference axis.

NOTE

escape.

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 plan e (Z-axis fo r the ZX p lane). Thi s cy cle 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

G75X(U)_ Z(W)_ P(∆i) Q(∆k) R(∆d) 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 fi rs t 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 speci fi c ati on.) ∆i : Depth of cut in the direction of the second axis on the plane (X-axis for the ZX

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

plane) ∆d : Relief amount of the tool at the cutting bottom

Unit Diameter/radius programming

Depends on the increment system for

∆i

Depends on the increment system for

∆k

Depends on the increment system for

∆d

Radius programming Not required Allowed

Radius programming Not required Not allowed

Radius programming NOTE Allowed

Sign

Normally, specify a positive value for ∆d. When Z (W) and ∆k are omitted,

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

Decimal point

- 66 -

Page 83

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

∆d

(R)

(F)

∆i

∆k

(F)

(R)

U/2

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

(R) B

∆i

∆i’

(R)

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

Explanation

- Operations

A cycle operation of cutting by ∆i and return by e is repeated. When cutting reaches point B, the too l escapes by ∆d. Then, the tool returns in rapid traverse, moves to the direction of point C by ∆k, 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.

- 67 -

Page 84

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

G76 P(m) (r) (a) Q(∆dmin) R(d ) ;

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

P 02 12 60

∆dmin : Minimum cutting depth

L : Lead of thread

programming

input

Depends on the increment system for the reference axis.

4.2.7 Multiple Threading Cycle (G76)

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

Format

G76 X(U)_ Z(W)_ R(i ) P(k ) Q(∆d) 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.

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 ∆d : Depth of cut in 1st cut

Unit

∆dmin

Diameter/radius

Radius programming Not required Not allowed

Radius programming Not required Allowed

Sign

Decimal point

∆d

Radius programming Required Allowed

Radius programming Not required Not allowed

- 68 -

Page 85

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

(F)

(R)

U/2

∆d

(R)

d (finishing allowance)

Last finishing cycle

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

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.

Fig. 4.2.7 (c)

- 69 -

Page 86

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

NOTE

CAUTION

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

Explanation

- Operations

This cycle performs threading so that the length o f 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 in terpolation and FL feedrate for thr ead chamfering and the feedrate for retraction after chamfering are th e same as for thread chamfering with G92 (canned cycle).

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 <

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

- 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 (alway s specified with a plus sign) Depth of cut in the first cut (∆d): 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.

- 70 -

Page 87

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Outer diameter machining

Internal diameter machining

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

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

U/2

3(R)

4(R)

1(R)

2(F)

U/2

3(R)

4(R)

1(R)

2(F)

at |i|≤|U/2|

U/2

3(R)

4(R)

1(R)

2(F)

U/2

3(R)

4(R)

1(R)

2(F)

NOTE

are used for this cycle and G92 threading cycle.

Table 4.2.7 (a)

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

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

- Accelerat ion/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 settin gs of parameter No. 1 626 an d No. 1627 for the threading cycle are used.

- Time constant and FL feedrate for threading

- Thread chamf er ing

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.

Common parameters for specifying the amount and angle of thread chamfer ing

- 71 -

Page 88

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

parameter No. 1611

Parameter No.

1466

No. 1627), and retraction feedrate specified in parameter No. 1466.

No. 1627), and rapid traverse rate specified in parameter No. 1420.

(parameter No. 1420).

NOTE

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

- Retract ion 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

Uses the type of acceleration/deceleration after interpolat i on for threading,

0 Other than 0

0 0

time constant for threading (parameter No. 1626), FL feedrate (parameter

Uses the type of acceleration/deceleration after interpolat i on for threading, time constant for threading (parameter No. 1626), FL feedrate (parameter

Before retraction a check is made to see that the s pec i fied 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

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

Description

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

- Shifting the start angle

The threading start angle cannot be shifted. However, if the Series 15 format is used, the thread ing start angle can be shifted. Please refer to the "MEMORY OPERATION USING Series 15 FORMAT".

- Feed hold i n a t hr eading cycle

When the threading cycle retract function is not used, the behavior of feed hold is as follows:

- If the parameter No.5109#3=0 and FEED HOLD button is pressed and released in the threading, the

tool returns to start point (point A) and stops. If FEED HOLD is kept pressed, the tool stops at the vicinity of the end point of retraction (point E).

- If the parameter No.5109#3=1 and FEED HOLD button is pressed and released or kept pressed in the

threading, the tool stops at the end point of retraction (point E).

- Feed hold when the threading cycle retract function is used

When feed hold is applied during threading in a combined threading cycle (G76), the tool quick ly retract s in the same way as for the last chamfering in a threading cy cle and returns t o the start poi nt in the curr ent cycle. When cycle start is triggered, the multiple threading cycle resumes.

- 72 -

Page 89

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Feed hold is applied at this point

Start point in the current cycle

Ordinary cycle

Rapid traverse

Motion at feed hold

X-axis

Z-axis

Cutting feed

CAUTION

Another feed hold cannot be performed during retraction.

Fig. 4.2.7 (d)

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

- Inch t hr eadi ng

Inch threading specified with address E is not allowed.

- Tool nose radius compensation

Tool nose radius compensation cannot be applied.

Example

Fig. 4.2.7 (e)

- 73 -

Page 90

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

4.2.8 Restrictions on Multiple Repetitive Canned Cycle (G70-G76)

Programmed commands

- Program memory

Programs using G70, G71, G72, or G73 must be stored in the program memory. The use of the mode in which programs stored in the program memory are called for operation enables these programs to be executed in other than the MEM mode. Programs using G74, G75, or G76 need not be stored in the program memory.

- Blocks in which data related to a multiple repetitive canned cycle is specified

The addresses P, Q, X, Z, U, W, and R should be specified correctly for each block.

In a block in which G70, G71, G72, or G73 is specified, the following functions cannot be specified:

- Custom macro calls (simple call, modal call, and subprogram call)

- Blocks in which data related to a target figure is specified

In the block which is specified by address P of a G71, G72 or G73, G00 or G01 code in group 01 should be commanded. If it is not commanded, alarm PS0065, “G00/G01 IS NOT IN THE FIRST BLOCK OF SHAPE PROGRAM” is generated.

In blocks with sequence numbers between those specified at P and Q in G70, G71, G72, and G73, the following commands can be specified: (1) Dwell (G04) (2) G00, G01, G02, and G03 When a circular interpolation command (G02, G03) is used, there must be no radius difference between the start point and end point of the arc. If there is a radius difference, the target finishing figure may not be recognized correctly, resulting in a cutting error such as excessive cutting. (3) Custom macro branch and repeat command The branch destination must be between the seq uence numbers specified at P and Q, however. High-speed branch specified by bits 1 and 4 of parameter No. 6000 is invalid. No custom macro call (simple, modal, or subprogram call) cannot be specified. (4) Direct drawing dimension programming command and chamfering and corner R command Direct drawing dimension programming and chamfering and corner R require multiple blocks to be

specified. The block with the last sequence number specified at Q must not be an intermediate block

of these specified blocks.

When G70, G71, G72, or G73 is executed, the sequence number specified by address P and Q should not be specified twice or more in the same program. When #1 = 2500 is executed using a custom macro, 2500.000 is assigned to #1. In such a case, P#1 is equivalent to P2500.

- 74 -

Page 91

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Manual intervention

Cancellation

Example of G72

Relation with other functions

- Manual i ntervention

After manual intervention is performed with the manual absolute on command before the execution of a multiple repetitive canned cycles (G70 to G76) or after the stop of the execu tion, when a cycle operati on starts, the manual intervention amount is canceled ev en with an incremental cycle start command. When only the first plane axis is specified in G74 or only the second plane axis is specified in G74, h owever, the manual intervention amount is canceled only along the specified axis.

Fig. 4.2.8 (a)

- Int er r upt ion type macro

Any interruption type macro program cannot be executed during execution of a multiple repetitive canned cycle.

- Program r estart and tool retract and recover

These functions cannot be executed in a block in a multiple repetitive canned cycle.

- Axis name and second auxi liary functions

Even if address U, V, or W is used as an axis name or secon d auxiliar y fun ction, dat a specified at addr ess U, V, or W in a G71 to G73 block is assumed to be that for the multiple repetitive canned cycle.

- Tool nose radius compensation

- Multi-spindle control

When a spindle selection by address P o f multi-spindle control or the command by the extended spindle name is used, S code cannot be specified at the block of multiple repetitive canned cycle command (G71-G73). (The alarm PS5305 “ILLEGAL SPINDLE NUMBER” is issued.) In this case, instead of specifying S code at the block of multiple repetitive canned cycle command (G71-G73) is specified, specify S code before the multip le repetitive canned cycle command (G71-G73) block.

- 75 -

Page 92

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

R R R C C 1

2 6 10 3 4

5 7 8 9 11

Cutting feed

+X R R R C

C C 1 2 3 4 5 6 7 8 9

Cutting feed

4.2.9 Reducing path for Multiple Repetitive Canned Cycle

Overview

In multiple repetitive canned cycle, a path of cycle can be reduced.

Explanation

In stock removal in turning (G71) of multiple repetitive canned cycle, conventional pat h was as follows (Fig. 4.2.9 (a)).

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

2. Moving in the direction of the second axis on the plane (X-axis for the ZX plane) In this function, it directly moves from the retraction end point to the last turning start point (Fig. 4.2.9 (b), Fig. 4.2.9 (c)). The cycle time can be reduced because moving path is reduced. To use this function, set bit 6 (RPA) of parameter No. 5125 to 1.

Rapid traverse

R: Retraction end point C: Turning start point

Fig. 4.2.9 (a) Conventional operation

Movement from retraction end point to last turning star t point

In a start block in the program for a target figure, the movement from the retraction end point to the last turning start point is changed.

When a start block in the program for a target figure is G00 : Axes move from the retraction end point to the last turning start point by rapid traverse.

Fig. 4.2.9 (b) Operation when this function is effective (Start block in the program for a target figure is G00.)

Rapid traverse

R: Retraction end point C: Turning start point

- 76 -

Page 93

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

WARNING

parameter No.5126.

R R R C C C 1 2 3

10 4 5

6 7 8

When a start block in the program for a target figure is G01 : Axes move from the retraction end point by rapid traverse until becoming a value that the distance to the last turning start point is set to parameter No.5126. These move from there to the last turning start point by cutting feed.

Rapid traverse

Cutting feed

R: Retraction end point C: Turning start point

Fig. 4.2.9 (c) Operation when this function is effective (Start block in the program for a target figure is G01.)

Specify G01 in a start block in the program for a target figure when turning st art point is near the processing surface. The distance of cutting can be adjusted by

Effect of reducing cycle time

In this function, it is more effective in reducin g cycle time to assume a start block in the program for a target figure to be G00. Therefore, it is recommended that turning start point is separated from work pi ece, and it sp ecifies G00 in the start block in the program for a target figure.

Limitation

- This function is valid only when bit 1 (LRP) of parameter No. 1401 is 1.

- This function is valid only in stock removal in turning (G71) and stock removal in facing (G72) of

multiple repetitive canned cycle.

- This function is invalid in type II of multiple repetitive canned cycle.

4.3 CANNED CYCLE FOR DRILLING

Canned cycles for drillin g make it easier for the programmer to create programs. With a canned cycle, a frequently-used machining operation can be specified in a single block with a G function; without canned cycles, more than one block is required. In addition, the use of canned cycles can shorten the program to save memory. Table 4.3 (a) lists canned cycles for drilling.

- 77 -

Page 94

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

operation

G80 - - - -

Cancel

intermittent

spindle CCW

G85

Z axis

Cutting feed

Dwell

Cutting feed

Front boring cycle

Cutting feed /

intermittent

Spindle CCW

G89

X axis

Cutting feed

Dwell

Cutting feed

Side boring cycle

Operation 1

Operation 2

Point R level

Initial level

Operation 6

Operation 5

Operation 3

Operation 4

Rapid traverse

Feed

G code

Positioning axis

Drilling axis

G83, G84, G85

X axis, C axis

Z axis

G87, G88, G89

Z axis, C axis

X axis

Table 4.3 (a) Canned cycles for drilling

G code Drilling axis

Hole machining

Operation in the

bottom hole position

Retraction operation Applications

G83 Z axis

G84 Z axis Cutting feed

G87 X axis

G88 X axis Cutting feed

Cutting feed /

Dwell Rapid traverse F r ont drilling cycle

Dwell →

Dwell Rapid traverse Side drilling cycle

Dwell →

Cutting feed Front tapping cycle

Cutting feed Side tapping cycle

Explanation

The canned cycle for drilling consists of the following six operation sequences.

Operation 1 Positioning of X (Z) and C axis Operation 2 Rapid traverse up to point R level Operation 3 Hole machining Operation 4 Operation at the bottom of a hole Operation 5 Retraction to point R level Operation 6 Rapid traverse up to the initial level

- Positioning axis and drilling axis

The C-axis and X- or Z-axis are used as positioning axes. The X- or Z-axis, which is not used as a positioning axis, is used as a drilling axis. A drilling G code specifies positioning axes and a drilling axis as shown below. Although canned cycles include tappin g and boring cycl es as well as drilling cycles, in this chapter, only the term drilling will be used to refer to operations implemented with canned cycles.

Fig. 4.3 (a) Operation sequence of canned cycle for drilling

Table 4.3 (b) Positioning axis and drilling axis

- 78 -

Page 95

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

G98 (Return to initial level)

G99 (Return to point R level)

Initial level

Point R level

In the case of without ",D"

command, the clearance parameter

to be used

High-speed peck drilling cycle

No.5114

Peck drilling cycle

No.5115

G83.1

High-speed peck drilling cycle (FS15-T format)

No.5114

G83.5, G87.5

High-speed peck drilling cycle

No.5114

G83.6, G87.6

Peck drilling cycle

No.5115

High-speed peck rigid tαpping cycle

Peck rigid tapping cycle

G84.2

Rigid tapping cycle (FS15-T format)

No.5213

G83 and G87, G84 and G88, and G85 and G89 have the same function respectively except for axes specified as positioning axes and a drilling axis.

- Dril ling mode

G83 to G85/G87 to G89 are modal G codes and remain in effect until canceled. When in effect, the current state is the drilling mode. Once drilling data is specified in the drilling mode, the data is retained until modified or canceled. Specify all necessary drilling data at the beginning of canned cycles; when canned cycles are being performed, specify data modifications only. The feedrate specified at F is retained also after the d rilling cycle i s canceled. When Q data i s required, it must be specified in each block. Once specified, the M code used for C-axis cl amp/unclamp functions as a modal code. It is canceled by specifying G80.

- Return poi nt level

In G code system A, the tool returns to the initial level from the bottom of a hole. In G code system B or C, specifying G98 returns the tool to the initial level from the bottom of a hole and specifying G99 returns the tool to the point R level from the bottom of a hole. The following illustrates how the tool moves when G98 or G99 is specified (Fig. 4.3 (b)). Generally, G99 is used for the first drilling operation and G98 is used for the last drilling operation.

Fig. 4.3 (b)

- Clearance

Clearance is commanded with an address D with a comma. If the cycle is commanded without ",D" command, the clearance parameter will be valid. The cycles that can be commanded are as shown in Table 4.3 (c). If clearance is not programmed, use parameterized clearance. ",D" should be commanded in the block where the drilling operation is performed. It is memorized as a modal command during canned cycle for drilling. Decimal point input is possible for the ",D" command.

Table 4.3 (c) List of canned cycle for drilling which clearance can be commanded

G code Function

G83, G87

G84, G88

- 79 -

No.5213

Page 96

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

NOTE

For K, specify an integer of 0 or 1 to 9999.

Positioning (rapid traverse G00)

Cutting feed (linear interpolation G01)

Dwell specified in the program

Dwell specified in parameter No.5111

(The value of α is specified with parameter No. 5110.)

M (α + 1)

Issuing the M code for C-axis unclamp

- Number of r epeat s

To repeat drilling for equally-spaced holes, specify the number of repeats in K_. K is effective only within the block where it is specified. Specify the first hole position in incremental programming. If it is specified in absolute programming, drilling is repeated at the same position.

Number of repeats K The maximum command value = 9999

When K0 is specified, drilling data is just stored without drilling being performed.

- M code used f or C-axis clamp/unclamp

When an M code specified in parameter No. 5110 for C-axis clamp/unclamp is coded in a program, the following operations occur. (1) The CNC issues the M code for C-axis clamp after the tool is positioned and while the tool is being

fed in rapid traverse to the point-R level.

(2) The CNC issues the M code for C-axis unclamp (the M code for C-axis clamp +1) after the tool

retracts to the point-R level.

(3) After the CNC issues the M code for C-axis unclamp, the tool dwells for the time specified in

parameter No. 5111.

- Cancel

To cancel a canned cycle, use G80 or a gro up 01 G code.

Group 01 G codes (Example) G00 : Positioning (rapid traverse) G01 : Linear interpolation G02 : Circular interpolation (CW) G03 : Circular interpolation (CCW)

- Symbols in figures

Subsequent subsections explain the individual canned cycles. Figures in these explanations use the following symbols:

Mα Issuing the M code for C-axis clamp

- 80 -

Page 97

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

CAUTION

is used for point R data.

1 In each canned cycle, addresses R, Z, and X are handled as follows:

R_ : Always handled as a radius. Z_ or X_ : Depends on diameter/radius programming.

2 For the B or C G-code system, G90 or G91 can be used to select an incremental

or absolute programming for hole position data (X, C or Z, C), the distance from point R to the bottom of the hole (Z or X), and the distance from the initial level to the point R level (R).

3 For canned cycles for drilling specified in the Series 15 format (by setting bit 1

(FCV) of parameter No. 0001 to 1 and bit 3 (F16) of parameter No. 5102 to 0), incremental programming is used for point R data when bit 6 (RAB) of parameter No. 5102 is set to 0.

When bit 6 (RAB) of parameter No. 5102 is set to 1, in G code system A,

absolute programming is used, and in G code system B or C, absolute or incremental programming is used according to G90 or G91.

For canned cycles for drilling in the Series 16 format, incremental programming

4.3.1 Front Drilling Cycle (G83)/Side Drilling Cycle (G87)

The peck drilling cycle or high-speed peck drilling cycle is used depending on the setting in RTR, bit 2 of parameter No. 5101. If depth of cut for each drilling is not specified, the normal drilling cycle is used. Without using parameter RTR, the high-speed peck drilling cycle can be specified with G83.5 or G87.5 and the peck drilling cycle can be specified with G83.6 or G87.6.

- High-speed peck drilling cycle (G83, G87) (bit 2 (RTR) of parameter No. 5101

This cycle performs high-speed peck drilling. The drill repeats the cycle of drilling at the cutting feedrate and retracting the specified retraction distance intermittently to the bottom of a hole. The drill draws cutting chips out of the hole when it retracts.

=0)

- 81 -

Page 98

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

G83 X(U)_ C(H)_ Z(W)_ R_ P_ Q_ ,D_ F_ K_ M_ ;

M_ : M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode)

G83 or G87 (G99 mode)

Mα

M (α + 1), P2

Point R

qqq

Point Z

Initial level

Point R level

Point R

Point Z

M (α + 1), P2

Format

G87 Z(W)_ C(H)_ X(U)_ R_ P_ Q_ ,D_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data Z_ or X_ : The distance from point R to the bottom of the hole R_ : The distance from the initial level to point R level P_ : Dwell time at the bottom of a hole Q_ : Depth of cut for each cutting feed ,D_ : Clearance F_ : Cutting feedrate K_ : Number of repeats (When it is needed)

Mα : M code for C-axis clamp M (α + 1) : M code for C-axis unclamp P1 : Dwell specified in the program P2 : Dwell specified in parameter No. 5111 d : Retraction distance specified in ",D" command or parameter No. 5114 q : Depth of cut

- 82 -

Page 99

B-64694EN-1/01 PROGRAMMING

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

G83 X(U)_ C(H)_ Z(W)_ R_ P_ Q_ ,D_ F_ K_ M_ ;

M_ : M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode)

G83 or G87 (G99 mode)

Point R

qqqdPoint Z

Initial level

MαP1M (α + 1), P2

Point R

qqqdPoint Z

Point R level

Mα

M (α + 1), P2

NOTE

performed. (See the description of the drilling cycle.)

- Peck dril ling cycle (G83, G87) (bit 2 (RTR) of parameter No. 5101 =1)

Format

G87 Z(W)_ C(H)_ X(U)_ R_ P_ Q_ ,D_ F_ K_ M_ ;

Mα : M code for C-axis clamp M (α + 1) : M code for C-axis unclamp P1 : Dwell specified in the program P2 : Dwell specified in parameter No. 5111 d : Clearance value specified in ",D" command or parameter No. 5115 q : Depth of cut

Example

M51 ; Setting C-axis index mode ON M3 S2000 ; Rotating the drill G00 X50.0 C0.0 ; Positioning the drill along the X- and C-axes G83 Z-40.0 R-5.0 Q5000 F5.0 M31 ; Drilling hole 1 C90.0 Q5000 M31 ; Drilling hole 2 C180.0 Q5000 M31 ; Drilling hole 3 C270.0 Q5000 M31 ; Drilling hole 4 G80 M05 ; Canceling the drilling cycle and stopping drill rotation M50 ; Setting C-axis index mode off

If the depth of cut for each cutting feed (Q) is not comm anded, normal drilling is

- 83 -

Page 100

PROGRAMMING B-64694EN-1/01

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

G83 X(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ;

M_ : M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode)

G83 or G87 (G99 mode)

Initial level

Point R

Point Z

Point R level

M (α + 1), P2

Mα

Point R level

Point R

Point Z

M (α + 1), P2

Mα

- Dril ling cycle (G83 or G87)

If depth of cut (Q) is not specified for each drilling, the normal drilling cycle is used. The tool is then

retracted from the bottom of the hole in rapid traverse.

Format

G87 Z(W)_ C(H)_ X(U)_ R_ P_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data Z_ or X_ : The distance from point R to the bottom of the hole R_ : The distance from the initial level to point R level P_ : Dwell time at the bottom of a hole F_ : Cutting feedrate K_ : Number of repeats (When it is needed.)

Mα : M code for C-axis clamp M (α + 1) : M code for C-axis unclamp P1 : Dwell specified in the program P2 : Dwell specified in parameter No. 5111

Example

M51 ; Setting C-axis index mode ON M3 S2000 ; Rotating the drill G00 X50.0 C0.0 ; Positioning the drill along the X- and C-axes G83 Z-40.0 R-5.0 P500 F5.0 M31 ; Drilling hole 1 C90.0 M31 ; Drilling hole 2 C180.0 M31 ; Drilling hole 3 C270.0 M31 ; Drilling hole 4 G80 M05 ; Canceling the drilling cycle and stopping drill rotation M50 ; Setting C-axis index mode off

- 84 -

fanuc 0i-F Plus Operator’s Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

SAFETY PRECAUTION

TABLE OF CONTENTS

I. GENERAL

1 GENERAL

1.1 NOTES ON READING THIS MANUAL

1.2 NOTES ON VARIOUS KINDS OF DATA

II. PROGRAMMING

1 GENERAL

1.1 OFFSET

2 PREPARATORY FUNCTION (G FUNCTION)

3 INTERPOLATION FUNCTION

3.1 THREADING (G32)

3.2 CONTINUOUS THREADING

3.3 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)

4.2.8 Restrictions on Multiple Repetitive Canned Cycle (G70-G76)

4.2.9 Reducing path for Multiple Repetitive Canned Cycle

4.3 CANNED CYCLE FOR DRILLING

4.3.1 Front Drilling Cycle (G83)/Side Drilling Cycle (G87)