Fanuc 32i руководство по программированию - Большая энциклопедия инструкций и руководств

FANUC Series 30+-MODEL BFANUC Series 31+-MODEL BFANUC Series 32+-MODEL B

For Lathe System

OPERATOR’S MANUAL

B-64484EN-1/02

• No part of this manual may be reproduced in any form. • All specifications and designs are subject to change without notice. The products in this manual are controlled based on Japan’s “Foreign Exchange and Foreign Trade Law”. The export of Series 30i-B, Series 31i-B5 from Japan is subject to an export license by the government of Japan. Other models in this manual may also be subject to export controls. Further, re-export to another country may be subject to the license of the government of the country from where the product is re-exported. Furthermore, the product may also be controlled by re-export regulations of the United States government. Should you wish to export or re-export these products, please contact FANUC for advice. The products in this manual are manufactured under strict quality control. However, when a serious accident or loss is predicted due to a failure of the product, pay careful attention to safety.

In this manual we have tried as much as possible to describe all the various matters. However, we cannot describe all the matters which must not be done, or which cannot be done, because there are so many possibilities. Therefore, matters which are not especially described as possible in this manual should be regarded as “impossible”.

B-64484EN-1/02 SAFETY PRECAUTIONS

s-1

SAFETY PRECAUTIONS This section describes the safety precautions related to the use of CNC units. It is essential that these precautions be observed by users to ensure the safe operation of machines equipped with a CNC unit (all descriptions in this section assume this configuration). Note that some precautions are related only to specific functions, and thus may not be applicable to certain CNC units. Users must also observe the safety precautions related to the machine, as described in the relevant manual supplied by the machine tool builder. Before attempting to operate the machine or create a program to control the operation of the machine, the operator must become fully familiar with the contents of this manual and relevant manual supplied by the machine tool builder.

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

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

WARNING Applied when there is a danger of the user being injured or when there is a

danger of both the user being injured and the equipment being damaged if the approved procedure is not observed.

CAUTION

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

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

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

SAFETY PRECAUTIONS B-64484EN-1/02

s-2

GENERAL WARNINGS AND CAUTIONS

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

machine. Before starting a production run, ensure that the machine is operating correctly by performing a trial run using, for example, the single block, feedrate override, or machine lock function or by operating the machine with neither a tool nor workpiece mounted. Failure to confirm the correct operation of the machine may result in the machine behaving unexpectedly, possibly causing damage to the workpiece and/or machine itself, or injury to the user.

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

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

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

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

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

4 When using a tool compensation function, thoroughly check the direction and amount of compensation. Operating the machine with incorrectly specified data may result in the machine behaving unexpectedly, possibly causing damage to the workpiece and/or machine itself, or injury to the user.

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

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

6 Immediately after switching on the power, do not touch any of the keys on the MDI unit until the position display or alarm screen appears on the CNC unit.

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

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

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

B-64484EN-1/02 SAFETY PRECAUTIONS

s-3

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

technology. Some pixels may not be turned on or may remain on. This phenomenon is a common attribute of LCDs and is not a defect.

NOTE Programs, parameters, and macro variables are stored in nonvolatile 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 nonvolatile 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.

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

WARNING 1 Coordinate system setting If a coordinate system is established incorrectly, the machine may behave

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

2 Positioning by nonlinear interpolation When performing positioning by nonlinear interpolation (positioning by nonlinear

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

3 Function involving a rotation axis When programming polar coordinate interpolation or normal-direction

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

4 Inch/metric conversion Switching between inch and metric inputs does not convert the measurement

units of data such as the workpiece origin offset, parameter, and current position. Before starting the machine, therefore, determine which measurement units are being used. Attempting to perform an operation with invalid data specified may damage the tool, the machine itself, the workpiece, or cause injury to the user.

SAFETY PRECAUTIONS B-64484EN-1/02

s-4

WARNING 5 Constant surface speed control When an axis subject to constant surface speed control approaches the origin of

the workpiece coordinate system, the spindle speed may become excessively high. Therefore, it is necessary to specify a maximum allowable speed. Specifying the maximum allowable speed incorrectly may damage the tool, the machine itself, the workpiece, or cause injury to the user.

6 Stroke check After switching on the power, perform a manual reference position return as

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

7 Tool post interference check A tool post interference check is performed based on the tool data specified

during automatic operation. If the tool specification does not match the tool actually being used, the interference check cannot be made correctly, possibly damaging the tool or the machine itself, or causing injury to the user. After switching on the power, or after selecting a tool post manually, always start automatic operation and specify the tool number of the tool to be used.

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

versa, the machine may behave unexpectedly. 9 Plane selection If an incorrect plane is specified for circular interpolation, helical interpolation, or

a canned cycle, the machine may behave unexpectedly. Refer to the descriptions of the respective functions for details.

10 Torque limit skip Before attempting a torque limit skip, apply the torque limit. If a torque limit skip

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

11 Programmable mirror image Note that programmed operations vary considerably when a programmable

mirror image is enabled. 12 Compensation function If a command based on the machine coordinate system or a reference position

return command is issued in compensation function mode, compensation is temporarily canceled, resulting in the unexpected behavior of the machine.

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

B-64484EN-1/02 SAFETY PRECAUTIONS

s-5

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

WARNING 1 Manual operation When operating the machine manually, determine the current position of the tool

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

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

required. If the machine is operated without first performing manual reference position return, it may behave unexpectedly. Stroke check is not possible before manual reference position return is performed. An unexpected operation of the machine may damage the tool, the machine itself, the workpiece, or cause injury to the user.

3 Manual numeric command When issuing a manual numeric command, determine the current position of the

tool and workpiece, and ensure that the movement axis, direction, and command have been specified correctly, and that the entered values are valid.

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

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

applied causes the tool and table to move rapidly. Careless handling may damage the tool and/or machine, or cause injury to the user.

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

threading, rigid tapping, or other tapping, the speed cannot be predicted, possibly damaging the tool, the machine itself, the workpiece, or causing injury to the operator.

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

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

7 Workpiece coordinate system shift Manual intervention, machine lock, or mirror imaging may shift the workpiece

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

SAFETY PRECAUTIONS B-64484EN-1/02

s-6

WARNING 8 Software operator’s panel and menu switches Using the software operator’s panel and menu switches, in combination with the

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

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

9 RESET key Pressing the RESET key stops the currently running program. As a result, the

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

10 Manual intervention If manual intervention is performed during programmed operation of the

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

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

using custom macro system variable #3004. Be careful when operating the machine in this case.

12 Dry run Usually, a dry run is used to confirm the operation of the machine. During a dry

run, the machine operates at dry run speed, which differs from the corresponding programmed feedrate. Note that the dry run speed may sometimes be higher than the programmed feed rate.

13 Cutter and tool nose radius compensation in MDI mode Pay careful attention to a tool path specified by a command in MDI mode,

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

14 Program editing If the machine is stopped, after which the machining program is edited

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

B-64484EN-1/02 SAFETY PRECAUTIONS

s-7

WARNINGS RELATED TO DAILY MAINTENANCE

WARNING 1 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 electric shock hazard.

NOTE The CNC uses batteries to preserve the contents of its memory, because it must

retain data such as programs, offsets, and parameters even while external power is not applied.

If the battery voltage drops, a low battery voltage alarm is displayed on the machine operator’s panel or screen. When a low battery voltage alarm is displayed, replace the batteries within a week. Otherwise, the contents of the CNC’s memory will be lost.

Refer to the Section “Method of replacing battery” in the OPERATOR’S MANUAL (Common to Lathe/Machining Center System) for details of the battery replacement procedure.

WARNING

2 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 electric shock hazard.

NOTE The absolute pulse coder uses batteries to preserve its absolute position. If the battery voltage drops, a low battery voltage alarm is displayed on the

machine operator’s panel or screen. When a low battery voltage alarm is displayed, replace the batteries within a

week. Otherwise, the absolute position data held by the pulse coder will be lost. Refer to the FANUC SERVO MOTOR αi series Maintenance Manual for details

of the battery replacement procedure.

SAFETY PRECAUTIONS B-64484EN-1/02

s-8

WARNING 3 Fuse replacement Before replacing a blown fuse, however, it is necessary to locate and remove the

cause of the blown fuse. For this reason, only those personnel who have received approved safety and maintenance training may perform this work.

When replacing a fuse with the cabinet open, be careful not to touch the high-voltage circuits (marked and fitted with an insulating cover).

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

B-64484EN-1/02 TABLE OF CONTENTS

c-1

TABLE OF CONTENTS

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

I. GENERAL

1 GENERAL …………………………………………………………………………………..3 1.1 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 CONSTANT LEAD 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 Restrictions on Canned Cycles…………………………………………………………………….35

4.2 MULTIPLE REPETITIVE CANNED CYCLE (G70-G76) ………………………… 38 4.2.1 Stock Removal in Turning (G71) …………………………………………………………………39 4.2.2 Stock Removal in Facing (G72) …………………………………………………………………..51 4.2.3 Pattern Repeating (G73) ……………………………………………………………………………..55 4.2.4 Finishing Cycle (G70) ………………………………………………………………………………..58 4.2.5 End Face Peck Drilling Cycle (G74)…………………………………………………………….62 4.2.6 Outer Diameter / Internal Diameter Drilling Cycle (G75) ……………………………….64 4.2.7 Multiple Threading Cycle (G76) ………………………………………………………………….66 4.2.8 Restrictions on Multiple Repetitive Canned Cycle (G70-G76)…………………………71

4.3 CANNED CYCLE FOR DRILLING……………………………………………………… 74

TABLE OF CONTENTS B-64484EN-1/02

c-2

4.3.1 Front Drilling Cycle (G83)/Side Drilling Cycle (G87) ……………………………………77 4.3.2 Front Tapping Cycle (G84) / Side Tapping Cycle (G88)…………………………………80 4.3.3 Front Boring Cycle (G85) / Side Boring Cycle (G89) …………………………………….81 4.3.4 Canned Cycle for Drilling Cancel (G80)……………………………………………………….82 4.3.5 Canned Cycle for Drilling with M Code Output Improved………………………………82 4.3.6 Precautions to be Taken by Operator ……………………………………………………………83

4.4 IN-POSITION CHECK SWITCHING FOR DRILLING CANNED CYCLE….. 83 4.5 RIGID TAPPING……………………………………………………………………………… 90

4.5.1 FRONT FACE RIGID TAPPING CYCLE (G84) / SIDE FACE RIGID TAPPING CYCLE (G88) …………………………………………………………………………..90

4.5.2 Peck Rigid Tapping Cycle (G84 or G88) ………………………………………………………96 4.5.3 Canned Cycle Cancel (G80)………………………………………………………………………100 4.5.4 Override during Rigid Tapping ………………………………………………………………….100

4.5.4.1 Extraction override ……………………………………………………………………………… 100 4.5.4.2 Override signal …………………………………………………………………………………… 101

4.6 CANNED GRINDING CYCLE (FOR GRINDING MACHINE)………………… 103 4.6.1 Traverse Grinding Cycle (G71)………………………………………………………………….105 4.6.2 Traverse Direct Constant-Size Grinding Cycle (G72) …………………………………..107 4.6.3 Oscillation Grinding Cycle (G73) ………………………………………………………………109 4.6.4 Oscillation Direct Constant-Size Grinding Cycle (G74)………………………………..111

4.7 CHAMFERING AND CORNER R …………………………………………………….. 113 4.8 MIRROR IMAGE FOR DOUBLE TURRET (G68, G69) ……………………….. 119 4.9 DIRECT DRAWING DIMENSION PROGRAMMING…………………………… 120

5 COMPENSATION FUNCTION……………………………………………………126 5.1 TOOL OFFSET……………………………………………………………………………… 126

5.1.1 Tool Geometry Offset and Tool Wear Offset……………………………………………….126 5.1.2 T Code for Tool Offset ……………………………………………………………………………..127 5.1.3 Tool Selection………………………………………………………………………………………….127 5.1.4 Offset Number …………………………………………………………………………………………128 5.1.5 Offset ……………………………………………………………………………………………………..128 5.1.6 Y Axis Offset…………………………………………………………………………………………..131

5.1.6.1 Support of arbitrary axes for Y axis offset ……………………………………………… 131 5.1.7 Second Geometry Tool Offset……………………………………………………………………131 5.1.8 4th/5th Axis Offset …………………………………………………………………………………..134

5.2 OVERVIEW OF TOOL NOSE RADIUS COMPENSATION (G40-G42) ….. 136 5.2.1 Imaginary Tool Nose………………………………………………………………………………..136 5.2.2 Direction of Imaginary Tool Nose ……………………………………………………………..138 5.2.3 Offset Number and Offset Value………………………………………………………………..139 5.2.4 Workpiece Position and Move Command……………………………………………………140 5.2.5 Notes on Tool Nose Radius Compensation………………………………………………….145

5.3 OVERVIEW OF CUTTER COMPENSATION (G40-G42)…………………….. 148 5.4 DETAILS OF CUTTER OR TOOL NOSE RADIUS COMPENSATION…… 154

5.4.1 Overview ………………………………………………………………………………………………..154 5.4.2 Tool Movement in Start-up ……………………………………………………………………….158 5.4.3 Tool Movement in Offset Mode…………………………………………………………………164 5.4.4 Tool Movement in Offset Mode Cancel………………………………………………………183 5.4.5 Prevention of Overcutting Due to Cutter or Tool Nose Radius Compensation …189 5.4.6 Interference Check …………………………………………………………………………………..192

5.4.6.1 Operation to be performed if an interference is judged to occur ………………… 196 5.4.6.2 Interference check alarm function …………………………………………………………. 196 5.4.6.3 Interference check avoidance function …………………………………………………… 198

5.4.7 Cutter or Tool Nose Radius Compensation for Input from MDI …………………….203

B-64484EN-1/02 TABLE OF CONTENTS

c-3

5.5 VECTOR RETENTION (G38) ………………………………………………………….. 205 5.6 CORNER CIRCULAR INTERPOLATION (G39) …………………………………. 206 5.7 EXTENDED TOOL SELECTION ……………………………………………………… 208 5.8 AUTOMATIC TOOL OFFSET (G36, G37)…………………………………………. 211 5.9 COORDINATE SYSTEM ROTATION (G68.1, G69.1)…………………………. 214 5.10 ACTIVE OFFSET VALUE CHANGE FUNCTION BASED ON MANUAL

FEED …………………………………………………………………………………………… 218

6 MEMORY OPERATION USING Series 15 FORMAT…………………….222 6.1 ADDRESSES AND SPECIFIABLE VALUE RANGE FOR Series 15

PROGRAM FORMAT…………………………………………………………………….. 222 6.2 SUBPROGRAM CALLING ……………………………………………………………… 222 6.3 CANNED CYCLE…………………………………………………………………………… 223

6.3.1 Outer Diameter/Internal Diameter Cutting Cycle (G90) ………………………………..224 6.3.1.1 Straight cutting cycle …………………………………………………………………………… 224 6.3.1.2 Taper cutting cycle ……………………………………………………………………………… 225

6.3.2 Threading Cycle (G92)……………………………………………………………………………..226 6.3.2.1 Straight threading cycle ……………………………………………………………………….. 226 6.3.2.2 Taper threading cycle ………………………………………………………………………….. 229

6.3.3 End Face Turning Cycle (G94) ………………………………………………………………….232 6.3.3.1 Face cutting cycle ……………………………………………………………………………….. 232 6.3.3.2 Taper cutting cycle ……………………………………………………………………………… 233

6.3.4 How to Use Canned Cycles……………………………………………………………………….235 6.3.5 Canned Cycle and Tool Nose Radius Compensation…………………………………….236 6.3.6 Restrictions on Canned Cycles…………………………………………………………………..237

6.4 MULTIPLE REPETITIVE CANNED CYCLE ………………………………………. 240 6.4.1 Stock Removal in Turning (G71) ……………………………………………………………….241 6.4.2 Stock Removal in Facing (G72) …………………………………………………………………253 6.4.3 Pattern Repeating (G73) ……………………………………………………………………………257 6.4.4 Finishing Cycle (G70) ………………………………………………………………………………260 6.4.5 End Face Peck Drilling Cycle (G74)…………………………………………………………..264 6.4.6 Outer Diameter / Internal 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……………………………………………………. 276 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) ………………………………………………………………………………….287 6.5.8 Canned Cycle for Drilling Cancel (G80)……………………………………………………..288 6.5.9 Precautions to be Taken by Operator ………………………………………………………….288

7 MUITI-PATH CONTROL FUNCTION…………………………………………..289 7.1 BALANCE CUT (G68, G69)…………………………………………………………….. 289

III. OPERATION

1 DATA INPUT/OUTPUT ……………………………………………………………..297

TABLE OF CONTENTS B-64484EN-1/02

c-4

1.1 INPUT/OUTPUT ON EACH SCREEN ………………………………………………. 297 1.1.1 Inputting and Outputting Y-axis Offset Data ……………………………………………….297

1.1.1.1 Inputting Y-axis offset data ………………………………………………………………….. 297 1.1.1.2 Outputting Y-axis Offset Data………………………………………………………………. 298

1.1.2 Inputting and Outputting Tool Offset / 2nd Geometry Data …………………………..299 1.1.2.1 Inputting tool offset / 2nd geometry data………………………………………………… 299 1.1.2.2 Outputting tool offset / 2nd geometry data ……………………………………………… 300

1.1.3 Inputting and Outputting 4th/5th Axis Offset Data……………………………………….300 1.1.3.1 Inputting 4th/5th axis offset data …………………………………………………………… 300 1.1.3.2 Outputting 4th/5th Axis Offset Data………………………………………………………. 301

1.2 INPUT/OUTPUT ON THE ALL IO SCREEN………………………………………. 303 1.2.1 Inputting and Outputting Y-axis Offset Data ……………………………………………….304 1.2.2 Inputting and Outputting Tool Offset / 2nd Geometry Tool Offset …………………305

2 SETTING AND DISPLAYING DATA……………………………………………307 2.1 SCREENS DISPLAYED BY FUNCTION KEY …………………………….. 307

2.1.1 Setting and Displaying the Tool Offset Value ……………………………………………..307 2.1.2 Direct Input of Tool Offset Value ………………………………………………………………312 2.1.3 Direct Input of Tool Offset Value Measured B…………………………………………….315 2.1.4 Counter Input of Offset value…………………………………………………………………….317 2.1.5 Setting the Workpiece Coordinate System Shift Value………………………………….318 2.1.6 Setting Tool Offset/Second Geometry Tool Offset Values…………………………….321 2.1.7 Setting the Y-Axis Offset ………………………………………………………………………….324 2.1.8 Setting the 4th/5th Axis Offset …………………………………………………………………..330 2.1.9 Chuck and Tail Stock Barriers …………………………………………………………………..335

APPENDIX

A PARAMETERS…………………………………………………………………………345 A.1 DESCRIPTION OF PARAMETERS………………………………………………….. 345 A.2 DATA TYPE………………………………………………………………………………….. 382 A.3 STANDARD PARAMETER SETTING TABLES………………………………….. 383

I. GENERAL

B-64484EN-1/02 GENERAL 1.GENERAL

— 3 —

1 GENERAL This manual consists of the following parts:

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

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

restrictions. III. OPERATION Describes the manual operation and automatic operation of a machine, procedures for inputting and

outputting data, and procedures for editing a program. APPENDIX Lists parameters.

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

control type. For other functions not specific to the lathe system, refer to the Operator’s Manual (Common to Lathe System/Machining Center System) (B-63484EN).

2 Some functions described in this manual may not be applied to some products. For detail, refer to the DESCRIPTIONS manual (B-64482EN).

3 This manual does not detail the parameters not mentioned in the text. For details of those parameters, refer to the Parameter Manual (B-64490EN).

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

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 machine tool builder.

Applicable models

This manual describes the models indicated in the table below. In the text, the abbreviations indicated below may be used.

Model name Abbreviation FANUC Series 30i-B 30i –B Series 30i FANUC Series 31i-B 31i –B FANUC Series 31i-B5 31i –B5

Series 31i

FANUC Series 32i-B 32i –B Series 32i

NOTE 1 Unless otherwise noted, the model names 31i-B, 31i-B5, and 32i-B are

collectively referred to as 30i. However, this convention is not necessarily observed when item 3 below is applicable.

2 Some functions described in this manual may not be applied to some products. For details, refer to the Descriptions (B-64482EN).

1.GENERAL GENERAL B-64484EN-1/02

— 4 —

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 30i- MODEL B Series 31i- MODEL B Series 32i- MODEL B

The following table lists the manuals related to Series 30i-B, Series 31i-B, Series 32i-B. This manual is indicated by an asterisk(*).

Table 1 (a) Related manuals Manual name Specification number

DESCRIPTIONS B-64482EN CONNECTION MANUAL (HARDWARE) B-64483EN CONNECTION MANUAL (FUNCTION) B-64483EN-1 OPERATOR’S MANUAL (Common to Lathe System/Machining Center System) B-64484EN OPERATOR’S MANUAL (For Lathe System) B-64484EN-1 * OPERATOR’S MANUAL (For Machining Center System) B-64484EN-2 MAINTENANCE MANUAL B-64485EN PARAMETER MANUAL B-64490EN 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

B-63874EN

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 Dual Check Safety Dual Check Safety CONNECTION MANUAL B-64483EN-2

B-64484EN-1/02 GENERAL 1.GENERAL

— 5 —

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

Table 1 (b) Related manuals Manual name Specification number

FANUC AC SERVO MOTOR αi series DESCRIPTIONS B-65262EN FANUC AC SPINDLE MOTOR αi series DESCRIPTIONS B-65272EN FANUC AC SERVO MOTOR βi series DESCRIPTIONS B-65302EN FANUC AC SPINDLE MOTOR βi series DESCRIPTIONS B-65312EN FANUC SERVO AMPLIFIER αi series DESCRIPTIONS B-65282EN FANUC SERVO AMPLIFIER βi series DESCRIPTIONS B-65322EN FANUC SERVO MOTOR αis series FANUC SERVO MOTOR αi series FANUC AC SPINDLE MOTOR αi series FANUC SERVO AMPLIFIER αi series MAINTENANCE MANUAL

B-65285EN

FANUC SERVO MOTOR βis series FANUC AC SPINDLE MOTOR βi series FANUC SERVO AMPLIFIER βi series MAINTENANCE MANUAL

B-65325EN

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

B-65270EN

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

B-65280EN

The above servo motors and the corresponding spindles can be connected to the CNC covered in this manual. In the αi SV, αi SP, αi PS, and βi SV series, however, they can be connected only to 30 i-B-compatible versions. In the βi SVSP series, they cannot be connected. This manual mainly assumes that the FANUC SERVO MOTOR αi series of servo motor is used. For servo motor and spindle information, refer to the manuals for the servo motor and spindle that are actually connected.

1.GENERAL GENERAL B-64484EN-1/02

— 6 —

1.1 NOTES ON READING THIS MANUAL

CAUTION 1 The function of an CNC machine tool system depends not only on the CNC, but on

the combination of the machine tool, its magnetic cabinet, the servo system, the CNC, the operator’s panels, etc. It is too difficult to describe the function, programming, and operation relating to all combinations. This manual generally describes these from the stand-point of the CNC. So, for details on a particular CNC machine tool, refer to the manual issued by the machine tool builder, which should take precedence over this manual.

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

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

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

1.2 NOTES ON VARIOUS KINDS OF DATA

CAUTION Machining programs, parameters, offset data, etc. are stored in the CNC unit

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

II. PROGRAMMING

B-64484EN-1/02 PROGRAMMING 1.GENERAL

— 9 —

1 GENERAL Chapter 1, «GENERAL», consists of the following sections: 1.1 OFFSET ………………………………………………………………………………………………………………………………9

1.1 OFFSET

Explanation — Tool offset

Usually, several tools are used for machining one workpiece. The tools have different tool length. It is very troublesome to change the program in accordance with the tools. Therefore, the length of each tool used should be measured in advance. By setting the difference between the length of the standard tool and the length of each tool in the CNC (see Chapter, “Setting and Displaying Data” in the OPERATOR’S MANUAL (Common to Lathe System/Machining Center System)), machining can be performed without altering the program even when the tool is changed. This function is called tool offset.

Workpiece

Standardtool

Roughcuttingtool

Finishingtool

Groovingtool

Threadingtool

Fig. 1.1 (a) Tool offset

PROGRAMMING B-64484EN-1/02

— 10 —

2. PREPARATORY FUNCTION (G FUNCTION)

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

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

Z_ ; G01 is effective in this range. X_ ;

G00 Z_ ; G00 is effective in this range. X_ ;

G01 X_ ; :

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

Explanation 1. When the clear state (bit 6 (CLR) of parameter No. 3402) is set at power-up or reset, the modal G

codes are placed in the states described below. (1) The modal G codes are placed in the states marked with as indicated in Table. (2) G20 and G21 remain unchanged when the clear state is set at power-up or reset. (3) Which status G22 or G23 at power on is set by bit 7 (G23) of parameter No. 3402. However,

G22 and G23 remain unchanged when the clear state is set at reset. (4) The user can select G00 or G01 by setting bit 0 (G01) of parameter No. 3402. (5) The user can select G90 or G91 by setting bit 3 (G91) of parameter No. 3402. When G code system B or C is used in the lathe system, setting bit 3 (G91) of parameter No.

3402 determines which code, either G90 or G91, is effective. 2. G codes other than G10 and G11 are one-shot G codes. 3. When a G code not listed in the G code list is specified, or a G code that has no corresponding

option is specified, alarm PS0010 occurs. 4. Multiple G codes can be specified in the same block if each G code belongs to a different group. If

multiple G codes that belong to the same group are specified in the same block, only the last G code specified is valid.

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

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

7. G codes are indicated by group.

B-64484EN-1/02 PROGRAMMING

— 11 —

2.PREPARATORY FUNCTION(G FUNCTION)

Table 2 (a) G code list G code system

A B C Group Function

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

G02.2 G02.2 G02.2 Involute interpolation CW G02.3 G02.3 G02.3 Exponential interpolation CW G02.4 G02.4 G02.4 3-dimensional coordinate system conversion CW G03.2 G03.2 G03.2 Involute interpolation CCW G03.3 G03.3 G03.3 Exponential interpolation CCW G03.4 G03.4 G03.4

3-dimensional coordinate system conversion CCW G04 G04 G04 Dwell

G05 G05 G05 AI contour control (command compatible with high precision contour control), High-speed cycle machining, High-speed binary program operation

G05.1 G05.1 G05.1 AI contour control / Nano smoothing / Smooth interpolation G05.4 G05.4 G05.4

HRV3, 4 on/off G06.2 G06.2 G06.2 01 NURBS interpolation G07 G07 G07 Hypothetical axis interpolation

G07.1 (G107)

Cylindrical interpolation

G08 G08 G08 Advanced preview control G09 G09 G09 Exact stop G10 G10 G10 Programmable data input

G10.6 G10.6 G10.6 Tool retract and recover G10.9 G10.9 G10.9 Programmable switching of diameter/radius specification G11 G11 G11

Programmable data input mode cancel G12.1 (G112)

G12.1 (G112)

Polar coordinate interpolation mode

G13.1 (G113)

21 Polar coordinate interpolation cancel mode

G17 G17 G17 XpYp plane selection G17.1 G17.1 G17.1 Plane conversion function G18 G18 G18 ZpXp plane selection G19 G19 G19

YpZp plane selection G20 G20 G70 Input in inch G21 G21 G71

06 Input in mm

G22 G22 G22 Stored stroke check function on G23 G23 G23

09 Stored stroke check function off

G25 G25 G25 Spindle speed fluctuation detection off G26 G26 G26

08 Spindle speed fluctuation detection on

G27 G27 G27 Reference position return check G28 G28 G28 Return to reference position

G28.2 G28.2 G28.2 In-position check disable reference position return G29 G29 G29 Movement from reference position G30 G30 G30 2nd, 3rd and 4th reference position return

G30.1 G30.1 G30.1 Floating reference point return

G30.2 G30.2 G30.2 In-position check disable 2nd, 3rd, or 4th reference position return

G31 G31 G31 Skip function G31.8 G31.8 G31.8

EGB-axis skip

PROGRAMMING B-64484EN-1/02

— 12 —

2. PREPARATORY FUNCTION (G FUNCTION)

Table 2 (a) G code list G code system

A B C Group Function

G32 G33 G33 Threading G34 G34 G34 Variable lead threading G35 G35 G35 Circular threading CW

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

G37 G37 G37 Automatic tool offset (Z axis) (When bit 3 (G36) of parameter No. 3405 is set to 0)

G37.1 G37.1 G37.1 Automatic tool offset (X axis) (When bit 3 (G36) of parameter No. 3405 is set to 1)

G37.2 G37.2 G37.2 Automatic tool offset (Z axis) (When bit 3 (G36) of parameter No. 3405 is set to 1)

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

G39 G39 G39

Tool radius/tool nose radius compensation: corner rounding interpolation

G40 G40 G40 Tool radius/tool nose radius compensation : cancel G41 G41 G41 Tool radius/tool nose radius compensation : left G42 G42 G42 Tool radius/tool nose radius compensation : right

G41.2 G41.2 G41.2 3-dimensional cutter compensation : left (type 1)

G41.3 G41.3 G41.3 3-dimensional cutter compensation : (leading edge offset)

G41.4 G41.4 G41.4 3-dimensional cutter compensation : left (type 1) (FS16i-compatible command)

G41.5 G41.5 G41.5 3-dimensional cutter compensation : left (type 1) (FS16i-compatible command)

G41.6 G41.6 G41.6 3-dimensional cutter compensation : left (type 2) G42.2 G42.2 G42.2 3-dimensional cutter compensation : right (type 1)

G42.4 G42.4 G42.4 3-dimensional cutter compensation : right (type 1) (FS16i-compatible command)

G42.5 G42.5 G42.5 3-dimensional cutter compensation : right (type 1) (FS16i-compatible command)

G42.6 G42.6 G42.6

3-dimensional cutter compensation : right (type 2) G40.1 G40.1 G40.1 Normal direction control cancel mode G41.1 G41.1 G41.1 Normal direction control left on G42 .1 G42 .1 G42 .1

19 Normal direction control right on

G43 G43 G43 Tool length compensation + (Bit 3 (TCT) of parameter No. 5040 must be «1».)

G44 G44 G44 Tool length compensation — (Bit 3 (TCT) of parameter No. 5040 must be «1».)

G43.1 G43.1 G43.1 Tool length compensation in tool axis direction (Bit 3 (TCT) of parameter No. 5040 must be «1».)

G43.4 G43.4 G43.4 Tool center point control (type 1) (Bit 3 (TCT) of parameter No. 5040 must be «1».)

G43.5 G43.5 G43.5 Tool center point control (type 2) (Bit 3 (TCT) of parameter No. 5040 must be «1».)

G43.7 (G44.7)

Tool offset (Bit 3 (TCT) of parameter No. 5040 must be «1».)

G49 (G49.1)

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

G50 G92 G92 Coordinate system setting or max spindle speed clamp G50.3 G92.1 G92.1

00 Workpiece coordinate system preset

B-64484EN-1/02 PROGRAMMING

— 13 —

2.PREPARATORY FUNCTION(G FUNCTION)

Table 2 (a) G code list G code system

A B C Group Function

— G50 G50 Scaling cancel — G51 G51

18 Scaling

G50.1 G50.1 G50.1 Programmable mirror image cancel G51.1 G51.1 G51.1

22 Programmable mirror image

G50.2 (G250)

Polygon turning cancel

G51.2 (G251)

20 Polygon turning

G50.4 G50.4 G50.4 Cancel synchronous control G50.5 G50.5 G50.5 Cancel composite control G50.6 G50.6 G50.6 Cancel superimposed control G51.4 G51.4 G51.4 Start synchronous control G51.5 G51.5 G51.5 Start composite control G51.6 G51.6 G51.6 Start superimposed control G52 G52 G52 Local coordinate system setting G53 G53 G53 Machine coordinate system setting

G53.1 G53.1 G53.1 Tool axis direction control G53.6 G53.6 G53.6

Tool center point retention type tool axis direction control G54

(G54.1) G54

(G54.1) Workpiece coordinate system 1 selection

G55 G55 G55 Workpiece coordinate system 2 selection G56 G56 G56 Workpiece coordinate system 3 selection G57 G57 G57 Workpiece coordinate system 4 selection G58 G58 G58 Workpiece coordinate system 5 selection G59 G59 G59

Workpiece coordinate system 6 selection G54.4 G54.4 G54.4 26 Workpiece setting error compensation G60 G60 G60 00 Single direction positioning G61 G61 G61 Exact stop mode G62 G62 G62 Automatic corner override mode G63 G63 G63 Tapping mode G64 G64 G64

Cutting mode G65 G65 G65 00 Macro call G66 G66 G66 Macro modal call A

G66.1 G66.1 G66.1 Macro modal call B G67 G67 G67

12 Macro modal call A/B cancel

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

G68.1 G68.1 G68.1 Coordinate system rotation start or 3-dimensional coordinate system conversion mode on

G68.2 G68.2 G68.2 Tilted working plane command G68.3 G68.3 G68.3 Tilted working plane command by tool axis direction G68.4 G68.4 G68.4

Tilted working plane command (incremental multi-command)

G69 G69 G69 04 Mirror image off for double turret or balance cutting mode

cancel

G69.1 G69.1 G69.1 17 Coordinate system rotation cancel or 3-dimensional coordinate system conversion mode off

PROGRAMMING B-64484EN-1/02

— 14 —

2. PREPARATORY FUNCTION (G FUNCTION)

Table 2 (a) G code list G code system

A B C Group Function

G70 G70 G72 Finishing cycle G71 G71 G73 Stock removal in turning G72 G72 G74 Stock removal in facing G73 G73 G75 Pattern repeating cycle G74 G74 G76 End face peck drilling cycle G75 G75 G77 Outer diameter/internal diameter drilling cycle G76 G76 G78

Multiple-thread cutting cycle G71 G71 G72 Traverse grinding cycle G72 G72 G73 Traverse direct sizing/grinding cycle G73 G73 G74 Oscillation grinding cycle G74 G74 G75

Oscillation direct sizing/grinding cycle

G80 G80 G80 10 Canned cycle cancel for drilling Electronic gear box : synchronization cancellation

G80.4 G80.4 G80.4 Electronic gear box: synchronization cancellation G81.4 G81.4 G81.4

28 Electronic gear box: synchronization start

G80.5 G80.5 G80.5 Electronic gear box 2 pair: synchronization cancellation G81.5 G81.5 G81.5

27 Electronic gear box 2 pair: synchronization start

G81 G81 G81 Spot drilling (FS15-T format) Electronic gear box : synchronization start

G82 G82 G82 Counter boring (FS15-T format) G83 G83 G83 Cycle for face drilling

G83.1 G83.1 G83.1 High-speed peck drilling cycle (FS15-T format) G83.5 G83.5 G83.5 High-speed peck drilling cycle G83.6 G83.6 G83.6 Peck drilling cycle G84 G84 G84 Cycle for face tapping

G84.2 G84.2 G84.2 Rigid tapping cycle (FS15-T format) G85 G85 G85 Cycle for face boring G87 G87 G87 Cycle for side drilling

G87.5 G87.5 G87.5 High-speed peck drilling cycle G87.6 G87.6 G87.6 Peck drilling cycle G88 G88 G88 Cycle for side tapping G89 G89 G89

Cycle for side boring G90 G77 G20 Outer diameter/internal diameter cutting cycle G92 G78 G21 Threading cycle G94 G79 G24

01 End face turning cycle

G91.1 G91.1 G91.1 00 Maximum specified incremental amount check G96 G96 G96 Constant surface speed control G97 G97 G97

02 Constant surface speed control cancel

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

SV speed control mode ON G93 G93 G93 Inverse time feed G98 G94 G94 Feed per minute G99 G95 G95

05 Feed per revolution

— G90 G90 Absolute programming — G91 G91

03 Incremental programming

— G98 G98 Canned cycle : return to initial level — G99 G99

11 Canned cycle : return to R point level

B-64484EN-1/02 PROGRAMMING 3.INTERPOLATION FUNCTION

— 15 —

3 INTERPOLATION FUNCTION Chapter 3, «INTERPOLATION FUNCTION», consists of the following sections: 3.1 CONSTANT LEAD THREADING (G32) ……………………………………………………………………………..15 3.2 CONTINUOUS THREADING……………………………………………………………………………………………..18 3.3 MULTIPLE THREADING…………………………………………………………………………………………………..19

3.1 CONSTANT LEAD THREADING (G32) Tapered screws and scroll threads in addition to equal lead straight threads can be cut by using a G32 command. The spindle speed is read from the position coder on the spindle in real time and converted to a cutting feedrate for feed-per minute mode, which is used to move the tool.

Straight thread

Tapered screw Scroll thread

Fig. 3.1 (a) Thread types

Format

X axis

δ2α Start point

δ1

End point_

0Z axis

G32IP_F_; IP_: End point F _: Lead of the long axis (always radius programming)

Fig. 3.1 (b) Example of threading

Explanation

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

3.INTERPOLATION FUNCTION PROGRAMMING B-64484EN-1/02

— 16 —

Tapered thread

LZZ

α≤45° lead is LZα≥45° lead is LX

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 specifying the thread lead.

Table 3.1 (a) Ranges of lead sizes that can be specified Least command increment

Metric input 0.0001 to 500.0000 mm Inch input 0.000001 to 9.999999 inch

B-64484EN-1/02 PROGRAMMING 3.INTERPOLATION FUNCTION

— 17 —

Example

Z axis

X axis

δ2 δ1

30mm

The following values are used in programming :Thread lead :4mm

δ1=3mmδ2=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

δ2

δ1

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

δ1=2mmδ2=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 ;

φ50

φ43

φ14

2.Tapered threading

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

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

3 When the FEED HOLD button is pressed again in the first block after threading mode that does not specify threading (or the button has been held down), the tool stops immediately at the block that does not specify threading.

4 When threading is executed in the single block status, the tool stops after execution of the first block not specifying threading.

3.INTERPOLATION FUNCTION PROGRAMMING B-64484EN-1/02

— 18 —

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

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

However, when the mode is changed from one automatic operation mode to another, the tool stops after execution of the block not specifying threading as for the single block mode in Note 4.

6 When the previous block was a threading block, cutting will start immediately without waiting for detection of the one-spindle-rotation signal even if the present block is a threading block. (Example)

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

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

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

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

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

PS0509, “TOOL OFFSET COMMAND IS NOT AVAILABLE”, is issued.

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

G32G32

G32

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

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

B-64484EN-1/02 PROGRAMMING 3.INTERPOLATION FUNCTION

— 19 —

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

L : Lead

Fig. 3.3 (a) Multiple thread screws.

Format

(Constant lead threading) G32 IP _ F_ Q_ ;

IP : End point F_ : Lead in longitudinal direction

G32 IP _ Q_ ; Q_ : Threading start angle

Explanation

— Available threading commands G32: Constant lead threading G34: Variable lead threading G76: Multiple threading cycle G92: Threading cycle

Limitation — Start angle

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

— Start angle increment

The start angle (Q) increment is 0.001 degrees. Note that no decimal point can be specified. Example: For a shift angle of 180 degrees, specify Q180000. Q180.000 cannot be specified, because it contains a decimal point.

— Specifiable start angle range A start angle (Q) of between 0 and 360000 (in 0.001-degree units) can be specified. If a value

greater than 360000 (360 degrees) is specified, it is rounded down to 360000 (360 degrees).

— Multiple threading cycle (G76) For the G76 multiple threading cycle command, always use the FS15 tape format.

3.INTERPOLATION FUNCTION PROGRAMMING B-64484EN-1/02

— 20 —

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

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

B-64484EN-1/02 PROGRAMMING

— 21 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

4 FUNCTIONS TO SIMPLIFY PROGRAMMING Chapter 4, «FUNCTIONS TO SIMPLIFY PROGRAMMING», consists of the following sections: 4.1 CANNED CYCLE (G90, G92, G94)……………………………………………………………………………………..21 4.2 MULTIPLE REPETITIVE CANNED CYCLE (G70-G76) ………………………………………………………38 4.3 CANNED CYCLE FOR DRILLING …………………………………………………………………………………….74 4.4 IN-POSITION CHECK SWITCHING FOR DRILLING CANNED CYCLE ……………………………..83 4.5 RIGID TAPPING………………………………………………………………………………………………………………..90 4.6 CANNED GRINDING CYCLE (FOR GRINDING MACHINE)…………………………………………….103 4.7 CHAMFERING AND CORNER R……………………………………………………………………………………..113 4.8 MIRROR IMAGE FOR DOUBLE TURRET (G68, G69) ………………………………………………………119 4.9 DIRECT DRAWING DIMENSION PROGRAMMING ………………………………………………………..120

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

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

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

2 A canned cycle can be performed on any plane (including parallel axes for plane definition). When G-code system A is used, however, U, V, and W cannot be set as a parallel axis.

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

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

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

PROGRAMMING B-64484EN-1/02

— 22 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

4.1.1 Outer Diameter/Internal Diameter Cutting Cycle (G90) This cycle performs straight or taper cutting in the direction of the length.

4.1.1.1 Straight cutting cycle

Format G90X(U)_Z(W)_F_;

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

U_,W_ : Travel distance to the cutting end point (point A’ in the Fig. 4.1.1.1 (a)) in the direction of the length

F_ : Cutting feedrate

X/2

X axis

Z axis

2(F)3(F) 1(R)

4(R)

Z W

U/2A’

(R)….Rapid traverse(F) ….Cutting feed

Fig. 4.1.1.1 (a) Straight cutting cycle

Explanation

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

the plane (specified X-coordinate for the ZX plane) in rapid traverse. (2) Operation 2 moves the tool to the specified coordinate of the first axis on the plane (specified

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

(3) Operation 3 moves the tool to the start coordinate of the second axis on the plane (start X-coordinate for the ZX plane) in cutting feed.

(4) Operation 4 moves the tool to the start coordinate of the first axis on the plane (start Z-coordinate for the ZX plane) in rapid traverse. (The tool returns to the start point (A).)

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

cycle start button once.

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

B-64484EN-1/02 PROGRAMMING

— 23 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

4.1.1.2 Taper cutting cycle

Format G90 X(U)_Z(W)_R_F_;

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

U_,W_ : Travel distance to the cutting end point (point A’ in the Fig. 4.1.1.2 (a)) in the direction of the length

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

3(F)

X/2

4(R)

U/2 1(R)

Z axis

2(F) R

X axis

A ’

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

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.

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

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

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

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

cycle start button once.

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

PROGRAMMING B-64484EN-1/02

— 24 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Table 4.1.1.2 (a)

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)W

U/2 3(F)

4(R)

1(R)

2(F)

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

at |R|≤|U/2| 4. U > 0, W < 0, R < 0

at |R|≤|U/2|

U/2 3(F)

4(R)

1(R)

2(F)

U/2 3(F)

4(R)

1(R)

2(F)

— Canceling the mode

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

4.1.2 Threading Cycle (G92)

4.1.2.1 Straight threading cycle

Format G92 X(U)_Z(W)_F_Q_;

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

U_,W_ : Travel distance to the cutting end point (point A’ in the Fig. 4.1.2.1 (a)) in the direction of the length

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

B-64484EN-1/02 PROGRAMMING

— 25 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

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

Fig. 4.1.2.1 (a) Straight threading

Explanation

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

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

the plane (specified X-coordinate for the ZX plane) in rapid traverse. (2) Operation 2 moves the tool to the specified coordinate of the first axis on the plane (specified

Z-coordinate for the ZX plane) in cutting feed. At this time, thread chamfering is performed. (3) Operation 3 moves the tool to the start coordinate of the second axis on the plane (start X-coordinate

for the ZX plane) in rapid traverse. (Retraction after chamfering) (4) Operation 4 moves the tool to the start coordinate of the first axis on the plane (start Z-coordinate for

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

Notes on this threading are the same as in threading in G32. However, a stop by feed hold is as follows; Stop after completion of path 3 of threading cycle.

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

cycle start button once.

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

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

PROGRAMMING B-64484EN-1/02

— 26 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

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

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

NOTE Common parameters for specifying the amount and angle of thread chamfering

are used for this cycle and threading cycle with G76.

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

Table 4.1.2.1 (a) Bit 0 (CFR) of

parameter No. 1611 Parameter No.

1466 Description

0 Other than 0 Uses the type of acceleration/deceleration after interpolation for threading, time constant for threading (parameter No. 1626), FL feedrate (parameter No. 1627), and retraction feedrate specified in parameter No. 1466.

0 0 Uses the type of acceleration/deceleration after interpolation for threading, time constant for threading (parameter No. 1626), FL feedrate (parameter No. 1627), and rapid traverse rate specified in parameter No. 1420.

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

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

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

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

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

— Feed hold in a threading cycle When the threading cycle retract function is not used, the machine stops at the end point of retraction after chamfering (end point of operation 3) by feed hold applied during threading.

B-64484EN-1/02 PROGRAMMING

— 27 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

— Threading cycle retract When the «threading cycle retract» optional function is used, feed hold may be applied during threading (operation 2). In this case, the tool immediately retracts with chamfering and returns to the start point on the second axis (X-axis), then the first axis (Z-axis) on the plane.

Feed hold is effected here.

Start point

Ordinary cycle

Rapid traverse

Motion at feed hold

X axis

Z axis

Cutting feed

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

CAUTION Another feed hold cannot be made during retreat.

— Inch threading

Inch threading specified with address E is not allowed.

4.1.2.2 Taper threading cycle

Format G92 X(U)_Z(W)_R_F_Q_;

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

U_,W_ : Travel distance to the cutting end point (point A’ in the Fig. 4.1.2.2 (a)) in the direction of the length

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

PROGRAMMING B-64484EN-1/02

— 28 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Detailed chamfered thread

1(R)

Z axis

3(R)

4(R)

2(F)

U/2

X/2R

X axis

Approx. 45°

(The chamfered angle in the left figureis 45 degrees or less because of thedelay in the servo system.)

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

A’

Fig. 4.1.2.2 (a) Taper threading cycle

Explanation

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

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

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

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

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

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

B-64484EN-1/02 PROGRAMMING

— 29 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

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

cycle start button once.

Table 4.1.2.2 (a) 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)W

U/2 3(F)

4(R)

1(R)

2(F)

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

at |R|≤|U/2| 4. U > 0, W < 0, R < 0

at |R|≤|U/2|

U/2 3(F)

4(R)

1(R)

2(F)

U/2 3(F)

4(R)

1(R)

2(F)

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

— Acceleration/deceleration after interpolation for threading — Time constant and FL feedrate for threading — Thread chamfering — Retraction after chamfering — Shifting the start angle — Threading cycle retract — Inch threading

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

PROGRAMMING B-64484EN-1/02

— 30 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

4.1.3 End Face Turning Cycle (G94)

4.1.3.1 Face cutting cycle

Format G94 X(U)_Z(W)_F_;

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

U_,W_ : Travel distance to the cutting end point (point A’ in the Fig. 4.1.3.1 (a)) in the direction of the end face

F_ : Cutting feedrate

X axis

4(R )

X /2

3(F)

Z axis

1(R )

2(F)

(R ) … R apid traverse (F )…. C utting feed

U /2

A’

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).)

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

cycle start button once.

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

B-64484EN-1/02 PROGRAMMING

— 31 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

4.1.3.2 Taper cutting cycle

Format G94 X(U)_Z(W)_R_F_;

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

U_,W_ : Travel distance to the cutting end point (point A’ in the Fig. 4.1.3.2 (a)) in the direction of the end face

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

(R) … Rapid traverse(F) … Cutting feed4(R)

X/2

3(F)

Z axis

1(R)

2(F)U/2

X axis

A’

Fig. 4.1.3.2 (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 end face and the sign of the taper amount (address R). For the cycle in the Fig. 4.1.3.2 (a), a minus sign is added to the taper amount.

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

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

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

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

cycle start button once.

PROGRAMMING B-64484EN-1/02

— 32 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

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

Table 4.1.3.2 (a) Outer diameter machining Internal diameter machining

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

X1(R)

U/2

3(F)

4(R)2(F)

WRZ

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)

X W

U/2

3(F)

4(R)2(F)

1(R)

— 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.

— Straight cutting cycle (G90)

Shape ofproduct

Shape of material

B-64484EN-1/02 PROGRAMMING

— 33 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

— Taper cutting cycle (G90)

Shape of product

Shape of material

— Face cutting cycle (G94)

Shape of product

Shape of material

— Face taper cutting cycle (G94)

Shape of product

Shape of material

PROGRAMMING B-64484EN-1/02

— 34 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

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

Outer diameter/internal diameter cutting cycle (G90) Tool nose radius center path Offset direction

Total tool nose

Tool nose radiuscenter path

Programmed path

5 7

16 2

Total toolnose

Total tool nose

End face cutting cycle (G94)

Total tool nose

Tool nose radiuscenter path

Programmed path

5 7

1 6 2

Total toolnose

Total tool nose

Tool nose radius center path Offset direction

Threading cycle (G92) Tool nose radius compensation cannot be applied.

B-64484EN-1/02 PROGRAMMING

— 35 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Differences between this CNC and the FANUC Series 16i/18i/21i NOTE 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, refer to «FANUC Series 16i/18i/21i Operator’s Manual.»

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

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

0 8

5 7

1 6 2

0 8

5 7

1 6 2

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

4.1.6 Restrictions on Canned Cycles

Limitation — Modal

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

PROGRAMMING B-64484EN-1/02

— 36 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Example

Workpiece

161284

66X 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;

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

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

Example N003 T0101; : : N010 G90 X20.0 Z10.0 F0.2; N011 G00 T0202; ← Cancels the canned cycle mode. N012 G90 X20.5 Z10.0;

— Plane selection command

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

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

B-64484EN-1/02 PROGRAMMING

— 37 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

— Reset If a reset operation is performed during execution of a canned cycle when any of the following states for holding a modal G code of group 01 is set, the modal G code of group 01 is replaced with the G01 mode: • Reset state (bit 6 (CLR) of parameter No. 3402 = 0) • Cleared state (bit 6 (CLR) of parameter No. 3402 = 1) and state where the modal G code of group 01

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

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

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

1(R)

3(F)

4(R)2(F)

Manual intervention Cancellation

Example of G94

PROGRAMMING B-64484EN-1/02

— 38 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

4.2 MULTIPLE REPETITIVE CANNED CYCLE (G70-G76) The multiple repetitive canned cycle is canned cycles to make CNC programming easy. For instance, the data of the finish work shape describes the tool path for rough machining. And also, a canned cycles for the threading is available.

NOTE 1 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, V, and W cannot be set as a parallel axis.

B-64484EN-1/02 PROGRAMMING

— 39 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

4.2.1 Stock Removal in Turning (G71) There are two types of stock removals in turning : Type I and II. To use type II, the «multiple repetitive canned cycle 2» optional function is required.

Format ZpXp plane

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

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

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

XpYp plane G71 V(Δd) R(e) ; G71 P(ns) Q(nf) U(Δw) V(Δu) F(f ) S(s ) T(t ) ; N (ns) ; … N (nf) ; Δd : Depth of cut The cutting direction depends on the direction AA’. This designation is modal and is

not changed until the other value is designated. Also this value can be specified by the parameter No. 5132, and the parameter is changed by the program command.

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

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

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

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

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

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

Unit Diameter/radius programming Sign Decimal point input

Δd Depends on the increment system for the reference axis.

Radius programming Not

required Allowed

PROGRAMMING B-64484EN-1/02

— 40 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Unit Diameter/radius programming Sign Decimal point input

e Depends on the increment system for the reference axis.

Radius programming Not

required Allowed

Δu Depends on the increment system for the reference axis.

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

Required Allowed

Δw Depends on the increment system for the reference axis.

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

Required Allowed

(R)

(F)

Δu/2

Δd

A’

ΔW

Target figure

45° e

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

+Z e: Escaping amount

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 Δd (depth of cut), with the finishing allowance specified by Δu/2 and Δw left. After the last cutting is performed in the direction of the second axis on the plane (X-axis for the ZX plane), rough cutting is performed as finishing along the target figure. After rough cutting as finishing, the block next to the sequence block specified at Q is executed.

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

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

A and B are ineffective and those specified in G71 block or the previous block are effective. M and second auxiliary functions are treated in the same way as F, S, and T functions.

4 When an option of constant surface speed control is selected, G96 or G97 command specified in the move command between points A and B are ineffective, and that specified in G71 block or the previous block is effective.

— Target figure Patterns

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

B-64484EN-1/02 PROGRAMMING

— 41 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Both linear andcircular interpolationare possible

A’

U(+)…W(+)

A’

U(+)…W(-)

A’

B A

U(-)…W(+)

A’

U(-)…W(-)

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 first and second axes on

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

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

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

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

compensation is applied is checked. The following checks can also be made.

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

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

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

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

PROGRAMMING B-64484EN-1/02

— 42 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

— Types I and II Selection of type I or II

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

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

Selecting type I or II

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

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

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

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

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

plane) must be specified.

Example ZX plane G71 V10.0 R5.0 ; G71 P100 Q200….; N100 X(U)_ ; (Specifies only the second axis on the plane.) : ; : ; N200…………;

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

forming the plane (Z- and X-axes for the ZX plane). It must not have any pocket as shown in the Fig. 4.2.1 (c).

No pockets are allowed.

A’

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

B-64484EN-1/02 PROGRAMMING

— 43 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

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

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

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

Escaping amount e (specified in thecommand or parameter No. 5133)45°

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

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

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

— Type II C

(F)

Δu/2

Δd

A’

ΔW

Target figure

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

(R)

Δd

(F)

(R)(R)

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 Δd (depth of cut), with the finishing allowance specified by Δu/2 and Δw left. Type II differs from type I in cutting the workpiece along the figure after rough cutting in the direction of the first axis on the plane (Z-axis for the ZX plane). After the last cutting, the tool returns to the start point specified in G71 and rough cutting is performed as finishing along the target figure, with the finishing allowance specified by Δu/2 and Δw left. Type II differs from type I in the following points:

PROGRAMMING B-64484EN-1/02

— 44 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

(1) In the block with sequence number ns, the two axes forming the plane (X-axis (U-axis) and Z-axis (W-axis) for the ZX plane) must be specified. When you want to use type II without moving the tool along the Z-axis on the ZX plane in the first block, specify W0.

Example ZX plane G71 V10.0 R5.0; G71 P100 Q200…….; N100 X(U)_ Z(W)_ ; (Specifies the two axes forming the plane.) : ; : ; N200…………;

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

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

12310 . . .

Fig. 4.2.1 (f) Figure having pockets (type II) The figure must show monotone change in the direction of the first axis on the plane (Z-axis for the

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

Monotone change is notobserved along the Z-axis.

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

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

plane during cutting operation (including a vertex in an arc command), the cutting tool may contact the workpiece. For this reason, for a figure which does not show monotone change, alarm PS0064 or PS0329 is issued. If the movement does not show monotone change, but is very small, and it can be determined that the movement is not dangerous, however, the permissible amount can be specified in parameter No. 5145 to specify that the alarm is not issued in this case.

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

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

B-64484EN-1/02 PROGRAMMING

— 45 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Fig. 4.2.1 (h) Figure which can be machined (type II) (3) After turning, the tool cuts the workpiece along its figure and escapes in cutting feed.

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

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

Escaping after cutting

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

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

e (specified in the command orparameter No. 5133)45°

Bottom

Fig. 4.2.1 (j) Escaping from the bottom to the direction of 45 degrees (4) When a position parallel to the first axis on the plane (Z-axis for the ZX plane) is specified in a

block in the program for the target figure, it is assumed to be at the bottom of a pocket. (5) After all rough cutting terminates along the first axis on the plane (Z-axis for the ZX plane), the tool

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

Then, rough cutting is performed as finishing along the target figure. At this time, the tool passes through the point in the obtained position (to which depth of cut Δd is added) when returning to the start point.

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

PROGRAMMING B-64484EN-1/02

— 46 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Depth of cut Δd

Start point

Escaping operation afterrough cutting

Escaping operation after rough cuttingas finishing

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)

<1><2><3>

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

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

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

<3><2><1>

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

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).

B-64484EN-1/02 PROGRAMMING

— 47 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

28 30

2522

9 102

14 20

1319

5 1

611

1216

31 32

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

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

22 21•

g Rapid traverse

Escaping fromthe bottom

Cutting feed

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

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

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

terminates, the tool moves to the nearest but one pocket and starts cutting. 2 When the figure has a pocket, generally specify a value of 0 for Δw (finishing

allowance). Otherwise, the tool may dig into the wall on one side. 3 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).

— Tool nose radius compensation

PROGRAMMING B-64484EN-1/02

— 48 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

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.; G40;…………………………Specify this command after the program specifying a target finishing figure. When this cycle is specified in the tool nose radius compensation mode, offset is temporarily canceled during movement to the start point. Start-up is performed in the first block. Offset is temporarily canceled again at the return to the cycle start point after termination of cycle operation. Start-up is performed again according to the next move command. This operation is shown in the Fig. 4.2.1 (p).

Cycle start point

Start-up

Offset cancel

Start-up

Offset cancel

Fig. 4.2.1 (p)

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’.

Target figure program forwhich tool nose radiuscompensation is not applied

B A

A’

Tool nose center path when tool nose radiuscompensation is applied with G42

Position between A-A’ in which start-up isperformed

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

B-64484EN-1/02 PROGRAMMING

— 49 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Target figure program forwhich tool nose radiuscompensation is not applied

+ZTool nose center path when toolnose radius compensation isapplied with G42

B A

A’

Position betweenA-A’ in which start-up is performed

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

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

— Reducing the cycle time

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.

For the type I command

+Z : Rapid traverse can be selected. : The mode specified in the start block is followed.

Operation 1

Operation 2

Previous turning point

Current turning point

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.

PROGRAMMING B-64484EN-1/02

— 50 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

For the type II command

Operation 1

Operation 2

Previous turning point

Current turning point

B-64484EN-1/02 PROGRAMMING

— 51 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

4.2.2 Stock Removal in Facing (G72) This cycle is the same as G71 except that cutting is performed by an operation parallel to the second axis on the plane (X-axis for the ZX plane).

Format ZpXp plane

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

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

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

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

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

changed until the other value is designated. Also this value can be specified by the parameter No. 5132, and the parameter is changed by the program command.

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

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

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

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

or T function in this G72 block is effective.

Unit Diameter/radius programming Sign Decimal point input

Δd Depends on the increment system for the reference axis.

Radius programming Not

required Allowed

e Depends on the increment system for the reference axis.

Radius programming Not

required Allowed

PROGRAMMING B-64484EN-1/02

— 52 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Unit Diameter/radius programming Sign Decimal point input

Δu Depends on the increment system for the reference axis.

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

Required Allowed

Δw Depends on the increment system for the reference axis.

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

Required Allowed

A’

Δu/2

Δd

Tool path(F)

(R)

45°

(R)

(F)

Δw

Target figure

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

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

Explanation

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

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

A and B are ineffective and those specified in G72 block or the previous block are effective. M and second auxiliary functions are treated in the same way as F, S, and T functions.

4 When an option of constant surface speed control is selected, G96 or G97 command specified in the move command between points A and B are ineffective, and that specified in G72 block or the previous block is effective.

— Target figure Patterns

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

B-64484EN-1/02 PROGRAMMING

— 53 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Both linear and circularinterpolation are possible

+ZB

U(-)…W(+)…

A’

U(-)…W(-)…

A’

U(+)…W(+)…

A’

U(+)…W(-)…

A’

Fig. 4.2.2 (s) 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 first and second axes on the plane.

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

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

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

compensation is applied is checked. The following checks can also be made.

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

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

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

Enabled when bit 2 (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.

PROGRAMMING B-64484EN-1/02

— 54 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

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

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

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

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

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

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

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

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

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

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

plane (Z-axis for the ZX plane) and it may have concaves (pockets). The figure must show monotone change in the direction of the second axis on the plane (X-axis for the ZX plane), however.

(3) When a position parallel to the second axis on the plane (X-axis for the ZX plane) is specified in a block in the program for the target figure, it is assumed to be at the bottom of a pocket.

(4) After all rough cutting terminates along the second axis on the plane (X-axis for the ZX plane), the tool temporarily returns to the start point. Then, rough cutting as finishing is performed.

— Tool nose radius compensation See the pages on which G71 is explained.

— Reducing the cycle time See the pages on which G71 is explained.

B-64484EN-1/02 PROGRAMMING

— 55 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

4.2.3 Pattern Repeating (G73) This function permits cutting a fixed pattern repeatedly, with a pattern being displaced bit by bit. By this cutting cycle, it is possible to efficiently cut work whose rough shape has already been made by a rough machining, forging or casting method, etc.

Format ZpXp plane

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

N (ns) ; …

N (nf) ;

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

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

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

This designation is modal and is not changed until the other value is designated. Also this value can be specified by the parameter No. 5135, and the parameter is changed by the program command.

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

This designation is modal and is not changed until the other value is designated. Also this value can be specified by the parameter No. 5136, and the parameter is changed by the program command.

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

modal and is not changed until the other value is designated. Also, this value can be specified by the parameter No. 5137, and the parameter is changed by the program command.

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

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

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

PROGRAMMING B-64484EN-1/02

— 56 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Unit Diameter/radius programming Sign Decimal point input

Δi Depends on the increment system for the reference axis.

Radius programming Required Allowed

Δk Depends on the increment system for the reference axis.

Radius programming Required Allowed

Δu Depends on the increment system for the reference axis.

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

Required Allowed

Δw Depends on the increment system for the reference axis.

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

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

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

Δw

A’

Δu/2 Δi+Δu/2

DΔk+Δw

Δw

Δu/2

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

(R)

(R)A

(F)

Fig. 4.2.3 (t) 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 Δu/2 and Δw left.

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

respectively, the meanings of them are determined by the presence of addresses P and Q.

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

A and B are ineffective and those specified in G73 block or the previous block are effective. M and second auxiliary functions are treated in the same way as F, S, and T functions.

B-64484EN-1/02 PROGRAMMING

— 57 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

— Target figure Patterns

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

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

— Check function The following check can be made.

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

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

— Tool nose radius compensation

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

PROGRAMMING B-64484EN-1/02

— 58 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

4.2.4 Finishing Cycle (G70) After rough cutting by G71, G72 or G73, the following command permits finishing.

Format G70 P(ns) Q(nf) ; ns : Sequence number of the first block for the program of finishing shape. nf : Sequence number of the last block for the program of finishing shape.

Explanation

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

— Target figure Check function

The following check can be made.

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

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

— Storing P and Q blocks

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

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

cycles)

B-64484EN-1/02 PROGRAMMING

— 59 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

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

G71, G72, and G73 are erased after execution of G70. All stored memory addresses of P and Q blocks are also erased by a reset.

— Return to the cycle start point

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

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

regardless of the setting of bit 1 (LRP) of parameter No. 1401. Before executing a finishing cycle for a target figure with a pocket cut by G71 or

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

— Tool nose radius compensation

When using tool nose radius compensation, specify a tool nose radius compensation command (G41 or G42) before a multiple repetitive canned cycle command (G70) and specify the cancel command (G40) after the multiple repetitive canned cycle command (G70). Program example G42;…………………………Specify this command before a multiple repetitive canned cycle command. G70P10Q20; G40;…………………………Specify this command after a multiple repetitive canned cycle command. 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’.

PROGRAMMING B-64484EN-1/02

— 60 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Example

Stock removal in facing (G72)

(Diameter designation for X axis, metric input)

N010 G50 X220.0 Z190.0 ; N011 G00 X176.0 Z132.0 ; N012 G72 W7.0 R1.0 ; N013 G72 P014 Q019 U4.0 W2.0 F0.3 S550 ; N014 G00 Z56.0 S700 ; N015 G01 X120.0 W14.0 F0.15 ; N016 W10.0 ; N017 X80.0 W10.0 ; N018 W20.0 ; N019 X36.0 W22.0 ; N020 G70 P014 Q019 ; Escaping amount: 1.0 Finishing allowance (4.0 in diameter in the X direction, 2.0 in the Z direction)

φ12

φ 80

φ40

φ 160

20 2

Start point

Z axis

X axis

2010 60 10

190

2 10

B-64484EN-1/02 PROGRAMMING

— 61 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Pattern repeating (G73)

(Diameter designation, metric input)

φ80

φ180

Z axis

X axis

220

130

110

φ160

2 14

φ120

40 10 40 20 4010

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

PROGRAMMING B-64484EN-1/02

— 62 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

4.2.5 End Face Peck Drilling Cycle (G74) This cycle enables chip breaking in outer diameter cutting. If the second axis on the plane (X-axis (U-axis) for the ZX plane) and address P are omitted, operation is performed only along the first axis on the plane (Z-axis for the ZX plane), that is, a peck drilling cycle is performed.

Format G74R (e) ; G74X(U)_ Z(W)_ P(Δi) Q(Δk) R(Δd) F (f ) ; e : Return amount This designation is modal and is not changed until the other value is designated.

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

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

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

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

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

Unit Diameter/radius programming Sign Decimal point

input

e Depends on the increment system for the reference axis.

Radius programming Not required Allowed

Δi Depends on the increment system for the reference axis.

Radius programming Not required Not allowed

Δk Depends on the increment system for the reference axis.

Radius programming Not required Not allowed

Δd Depends on the increment system for the reference axis.

Radius programming NOTE Allowed

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

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

B-64484EN-1/02 PROGRAMMING

— 63 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

U/2

Δd

Δi’

Δk’ Δk Δk Δk Δk

(R)

(F)

(R) (R) (R) (F)

(F) (F)

(F)

Δi

[0 < Δk’ ≤ Δk]

X Z

(R)

[0 < Δi’ ≤ Δi]

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

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

Explanation — Operations

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

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

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

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

— Tool nose radius compensation Tool nose radius compensation cannot be applied.

PROGRAMMING B-64484EN-1/02

— 64 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

4.2.6 Outer Diameter / Internal Diameter Drilling Cycle (G75) This cycle is equivalent to G74 except that the second axis on the plane (X-axis for the ZX plane) changes places with the first axis on the plane (Z-axis for the ZX plane). This cycle enables chip breaking in end facing. It also enables grooving during outer diameter cutting and cutting off (when the Z-axis (W-axis) and Q are omitted for the first axis on the plane).

Format G75R (e) ; G75X(U)_ Z(W)_ P(Δi) Q(Δk) R(Δd) F (f ) ; e : Return amount This designation is modal and is not changed until the other value is designated.

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

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

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

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

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

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

Unit Diameter/radius programming Sign Decimal point input

e Depends on the increment system for the reference axis.

Radius programming Not required Allowed

Δi Depends on the increment system for the reference axis.

Radius programming Not required Not allowed

Δk Depends on the increment system for the reference axis.

Radius programming Not required Not allowed

Δd Depends on the increment system for the reference axis.

Radius programming NOTE Allowed

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

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

B-64484EN-1/02 PROGRAMMING

— 65 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Δd

(R)

(F) Δi

ZΔk

(F)

(R)

U/2

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

(R)

Δi

Δi’

(R)

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

Explanation

— Operations A cycle operation of cutting by Δi and return by e is repeated. When cutting reaches point B, the tool escapes by Δd. Then, the tool returns in rapid traverse, moves to the direction of point C by Δk, and performs cutting again. Both G74 and G75 are used for grooving and drilling, and permit the tool to relief automatically. Four symmetrical patterns are considered, respectively.

— Tool nose radius compensation Tool nose radius compensation cannot be applied.

PROGRAMMING B-64484EN-1/02

— 66 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

4.2.7 Multiple Threading Cycle (G76) This threading cycle performs one edge cutting by the constant amount of cut.

Format G76 P(m) (r) (a) Q(Δdmin) R(d ) ; G76 X(U)_ Z(W)_ R(i ) P(k ) Q(Δd) F (L ) ; m : Repetitive count in finishing (1 to 99) This value can be specified by the parameter No. 5142, and the parameter is changed by

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

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

a : Angle of tool nose One of six kinds of angle, 80°, 60°, 55°, 30°, 29°, and 0°, can be selected, and specified

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

m, r, and a are specified by address P at the same time. (Example) When m=2, r=1.2L, a=60°, specify as shown below (L is lead of thread).

P 02 12 60 a

r m

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

cutting depth is clamped at this value. This value can be specified by parameter No. 5140, and the parameter is changed by the program command.

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

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

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

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

Unit Diameter/radius programming Sign Decimal point

input

Δdmin Depends on the increment system for the reference axis.

Radius programming Not required Not allowed

d Depends on the increment system for the reference axis.

Radius programming Not required Allowed

i Depends on the increment system for the reference axis.

Radius programming Required Allowed

k Depends on the increment system for the reference axis.

Radius programming Not required Not allowed

B-64484EN-1/02 PROGRAMMING

— 67 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Unit Diameter/radius programming Sign Decimal point

input

Δd Depends on the increment system for the reference axis.

Radius programming Not required Not allowed

(F)

(R) A

U/2

Δd

i X

D k

(R)

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

Δd

Δd√n 1st

3rd 2nd

nth

Tool nose

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.

PROGRAMMING B-64484EN-1/02

— 68 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

d (finishing allowance)Last finishing cycle

Explanation — Operations

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

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

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

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

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

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

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

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

B-64484EN-1/02 PROGRAMMING

— 69 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Table 4.2.7 (a) 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) W

U/2 3(R)

4(R)

1(R)

2(F)

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

at |i|≤|U/2| 4. U > 0, W < 0, i < 0

at |i|≤|U/2|

U/2 3(R)

4(R)

1(R)

2(F)

U/2 3(R)

4(R)

1(R)

2(F)

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

NOTE Common parameters for specifying the amount and angle of thread chamfering

are used for this cycle and G92 threading cycle.

PROGRAMMING B-64484EN-1/02

— 70 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

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

Table 4.2.7 (b) Bit 0 (CFR) of parameter No.

1611

Parameter No. 1466 Description

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

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

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

— Shifting the start angle The threading start angle cannot be shifted.

— Feed hold in a threading cycle When the threading cycle retract function is not used, the machine stops at the end point of retraction after chamfering (point E on the cutting path for a multiple threading cycle) by feed hold applied during threading.

— Feed hold when the threading cycle retract function is used When the «threading cycle retract» optional function is used, feed hold may be applied during threading in a combined threading cycle (G76). In this case, the tool quickly retracts in the same way as for the last chamfering in a threading cycle and returns to the start point in the current cycle. When cycle start is triggered, the multiple threading cycle resumes.

Feed hold is applied at th is point

Start point in the current cycle

Ordinary cycle

Rapid traverse

Motion at feed hold

X-axis

Z-axis

Cutting feed

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

B-64484EN-1/02 PROGRAMMING

— 71 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

CAUTION

Another feed hold cannot be performed during retraction.

— Inch threading Inch threading specified with address E is not allowed.

— Tool nose radius compensation Tool nose radius compensation cannot be applied.

Example

G80 X80.0 Z130.0; G76 P011060 Q100 R200 ; G76 X60.64 Z25.0 P3680 Q1800 F6.0 ;

1.8

3.68

105 25

1.8

X axis

Z axis

ϕ68

ϕ60

.64

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)

PROGRAMMING B-64484EN-1/02

— 72 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

— 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 sequence 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.

Relation with other functions — Manual intervention

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 execution, when a cycle operation starts, the manual intervention amount is canceled even 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, however, the manual intervention amount is canceled only along the specified axis.

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

— Program restart and tool retract and recover These functions cannot be executed in a block in a multiple repetitive canned cycle.

Manual interventionCancellation

Example of G72

B-64484EN-1/02 PROGRAMMING

— 73 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

— Axis name and second auxiliary functions Even if address U, V, or W is used as an axis name or second auxiliary function, data specified at address 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 When using tool nose radius compensation, specify a tool nose radius compensation command (G41, G42) before a multiple repetitive canned cycle command (G70, G71, G72, G73) and specify the cancel command (G40) outside the programs (from the block specified with P to the block specified with Q) specifying a target finishing figure. If tool nose radius compensation is specified in the program specifying a target finishing figure, alarm PS0325, “UNAVAILABLE COMMAND IS IN SHAPE PROGRAM”, is issued.

PROGRAMMING B-64484EN-1/02

— 74 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

4.3 CANNED CYCLE FOR DRILLING Canned cycles for drilling 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.

Table 4.3 (a) Canned cycles for drilling

G code Drilling axis Hole machining

operation Operation in the

bottom hole position Retraction operation Applications

G80 — — — — Cancel

G83 Z axis Cutting feed / intermittent

Dwell Rapid traverse Front drilling cycle

G84 Z axis Cutting feed Dwell →

spindle CCW Cutting feed Front tapping cycle

G85 Z axis Cutting feed Dwell Cutting feed Front boring cycle

G87 X axis Cutting feed / intermittent

Dwell Rapid traverse Side drilling cycle

G88 X axis Cutting feed Dwell →

Spindle CCW Cutting feed Side tapping cycle

G89 X axis Cutting feed Dwell Cutting feed Side boring 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

Operation 1

Operation 2

Point R level

Initial level

Operation 6

Operation 5

Operation 3

Operation 4 Rapid traverseFeed

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

— 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.

B-64484EN-1/02 PROGRAMMING

— 75 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Although canned cycles include tapping and boring cycles as well as drilling cycles, in this chapter, only the term drilling will be used to refer to operations implemented with canned cycles.

Table 4.3 (b) Positioning axis and drilling axis G code Positioning axis Drilling axis

G83, G84, G85 X axis, C axis Z axis G87, G88, G89 Z axis, C axis X axis

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.

— Drilling 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 drilling cycle is canceled. When Q data is required, it must be specified in each block. Once specified, the M code used for C-axis clamp/unclamp functions as a modal code. It is canceled by specifying G80.

— Return point 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. The initial level does not change even when drilling is performed in the G99 mode.

G98 (Return to initial level) G99 (Return to point R level)

Initial level

Point R level

Fig. 4.3 (b)

— Number of repeats

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.

PROGRAMMING B-64484EN-1/02

— 76 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

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

— M code used for 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 group 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:

Positioning (rapid traverse G00) Cutting feed (linear interpolation G01)

P1 Dwell specified in the program P2 Dwell specified in parameter No.5111 Mα Issuing the M code for C-axis clamp

(The value of α is specified with parameter No. 5110.) M (α + 1) Issuing the M code for C-axis unclamp

CAUTION

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 is used for point R data.

B-64484EN-1/02 PROGRAMMING

— 77 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

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 the RTR parameter, 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 =0)

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.

Format G83 X(U)_ C(H)_ Z(W)_ R_ P_ Q_ F_ K_ M_ ; or G87 Z(W)_ C(H)_ X(U)_ R_ P_ Q_ 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 F_ : Cutting feedrate K_ : Number of repeats (When it is needed) 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), P2Point R

Point Z

Initial level

Point R levelPoint R

Point Z

M (α + 1), P2

Mα

PROGRAMMING B-64484EN-1/02

— 78 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

— Peck drilling cycle (G83, G87) (bit 2 (RTR) of parameter No. 5101 =1)

Format G83 X(U)_ C(H)_ Z(W)_ R_ P_ Q_ F_ K_ M_ ; or G87 Z(W)_ C(H)_ X(U)_ R_ P_ Q_ 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 F_ : Cutting feedrate K_ : Number of repeats (When it is needed.) M_ : M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode) G83 or G87 (G99 mode)

Point R

Point Z

Initial level

Mα

M (α + 1), P2

Point R

Point Z

Point R level

Mα

M (α + 1), P2

P1 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 parameter No. 5115

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

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

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

B-64484EN-1/02 PROGRAMMING

— 79 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

— Drilling 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 G83 X(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ; or 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.) 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 levelM (α + 1), P2

Mα

Point R levelPoint R

Point Z

M (α + 1), P2

Mα

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

PROGRAMMING B-64484EN-1/02

— 80 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

4.3.2 Front Tapping Cycle (G84) / Side Tapping Cycle (G88) This cycle performs tapping. In this tapping cycle, when the bottom of the hole has been reached, the spindle is rotated in the reverse direction.

Format G84 X(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ; or G88 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.) M_ : M code for C-axis clamp (when it is needed.)

G84 or G88 (G98 mode) G84 or G88 (G99 mode)

Point R

Point Z

Spindle CCW

Spindle CW

Initial level

M (α + 1), P2

Mα

Point R

Point Z

Spindle CCW

Spindle CW

Point R level

Mα

M (α + 1), P2

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

Explanation Tapping is performed by rotating the spindle clockwise. When the bottom of the hole has been reached, the spindle is rotated in the reverse direction for retraction. This operation creates threads. Feedrate overrides are ignored during tapping. A feed hold does not stop the machine until the return operation is completed.

NOTE Bit 3 (M5T) of parameter No. 5105 specifies whether the spindle stop command

(M05) is issued before the direction in which the spindle rotates is specified with M03 or M04. For details, refer to the operator’s manual created by the machine tool builder.

Example

M51 ; Setting C-axis index mode ON M3 S2000 ; Rotating the drill

B-64484EN-1/02 PROGRAMMING

— 81 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

G00 X50.0 C0.0 ; Positioning the drill along the X- and C- axes G84 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

4.3.3 Front Boring Cycle (G85) / Side Boring Cycle (G89) This cycle is used to bore a hole.

Format G85 X(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ; or G89 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.) M_ : M code for C-axis clamp (When it is needed.)

G85 or G89 (G98 mode) G85 or G89 (G99 mode)

Point R

Point Z

Initial level

M (α + 1), P2

Mα

Point R

Point Z

Point R level

Mα

M (α + 1), P2

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

Explanation After positioning, rapid traverse is performed to point R. Drilling is performed from point R to point Z. After the tool reaches point Z, it returns to point R at a feedrate twice the cutting feedrate.

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 G85 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

PROGRAMMING B-64484EN-1/02

— 82 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

G80 M05 ; Canceling the drilling cycle and stopping drill rotation M50 ; Setting C-axis index mode off

4.3.4 Canned Cycle for Drilling Cancel (G80) G80 cancels canned cycle for drilling.

Format G80 ;

Explanation

Canned cycle for drilling is canceled to perform normal operation. Point R and point Z are cleared. Other drilling data is also canceled (cleared).

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

4.3.5 Canned Cycle for Drilling with M Code Output Improved

Overview Up to two pairs of M codes used for C-axis clamp/unclamp in canned cycles for drilling can be set for each path.

Details Set the M codes for C-axis clamp/unclamp in the following parameters.

Bit 4 of parameter No. 5161=1 Pair 1 Pair 2

Bit 4 of parameter No. 5161=0

M code for clamp No.5110 No.13544 No.5110 M code for unclamp No.13543 No.13545 (Setting in parameter No. 5110 + 1)

When the M code for clamp set in parameter No. 5110 or 13544 (valid when bit 4 (CME) of parameter No. 5161 is set to 1) is specified in the block for a canned cycle for drilling, the specified M code is output before the tool is fed in rapid traverse to the point-R level after positioned. The M code for unclamp paired with that specified M code is output after the tool retracts to the point-R level. Example 1: When bit 4 of parameter No. 5161 is set to 1, and 68, 78, 168, and 178 are specified in parameters

Nos. 5110, 13543, 13544, 13545, respectively, the following M codes are output. Command Clamp Unclamp

G83X_C_…M68 M68 M78 G83X_C_…M168 M168 M178

B-64484EN-1/02 PROGRAMMING

— 83 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Example 2: When bit 4 of parameter No. 5161 is set to 0, and 68 is specified in parameter No. 5110, respectively,

the following M codes are output. Command Clamp Unclamp

G83X_C_…M68 M68 M69

NOTE 1 Both the M codes for clamp and unclamp are set to 0, the setting of the pair is

invalid. 2 If the same M code for clamp is set for pairs 1 and 2, the setting for pair 1 that is

specified in parameter No. 13543 is used as the M code for unclamp.

4.3.6 Precautions to be Taken by Operator

— Reset and emergency stop Even when the controller is stopped by resetting or emergency stop in the course of drilling cycle, the drilling mode and drilling data are saved; with this mind, therefore, restart operation.

— Single block When drilling cycle is performed with a single block, the operation stops at the end points of operations 1, 2, 6 in Fig. 4.3 (a). Consequently, it follows that operation is started up 3 times to drill one hole. The operation stops at the end points of operations 1, 2 with the feed hold lamp ON. If there is a remaining repetitive count at the end of operation 6, the operation is stopped by feed hold. If there is no remaining repetitive count, the operation is stopped in the single block stop state.

— Feed hold When «Feed Hold» is applied between operations 3 and 5 by G84/G88, the feed hold lamp lights up immediately if the feed hold is applied again to operation 6.

— Override During operation with G84 and G88, the feedrate override is 100%.

4.4 IN-POSITION CHECK SWITCHING FOR DRILLING CANNED CYCLE

Overview This function enables dedicated in-position widths to be used for drilling canned cycle. Up to four different dedicated in-position widths are available, one for hole bottoms and three for other than hole bottoms. Using a little large in-position width for operations at locations where no nigh precision is required makes drilling canned cycle faster.

Explanation Setting bit 4 (ICS) of parameter No. 5107 to 1 enables dedicated in-position widths to be used for drilling canned cycle. Up to four different dedicated in-position widths are available, one for hole bottoms and three for other than hole bottoms. In conventional drilling canned cycle, the same operation is performed for both in-position checks between cycles for locations where no very high precision is required (A in Fig. 4.4 (a)) and in-position checks between cycles for hole bottoms where a high precision is required (B in Fig. 4.4 (a)) because the same in-position width is used for all cycles.

PROGRAMMING B-64484EN-1/02

— 84 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Using this function makes it possible to reduce the time needed to get in an in-position state (to reduce the necessary cycle time) by setting a small in-position width for hole bottoms so as to assure a high precision while setting a little large in-position width for other than hole bottoms.

Fig. 4.4 (a) Example of a peck drilling cycle (G83)

— Parameters related to in-position widths

This function uses the following in-position widths. In-position width for other than hole bottoms (regular) (parameter No. 5184) In-position width for other than hole bottoms (for retraction in peck drilling cycle) (parameter No.

5185) In-position width for other than hole bottoms (for shift in boring cycles (G76 and G87) (parameter

No. 5186) In-position width for hole bottoms (parameter No. 5187)

— Supported drilling canned cycle

The following table lists the drilling canned cycle for which this function is usable.

T Table 4.4 (a) Drilling canned cycle for which this function is usable (lathe system)

G code Use G83 High-speed peck drilling cycle

G83.5 Front high-speed peck drilling cycle G83.6 Front peck drilling cycle G84 Front tapping cycle G85 Front boring cycle G87 Side drilling cycle

G87.5 Side high-speed peck drilling cycle G87.6 Side peck drilling cycle G88 Side tapping cycle G89 Side boring cycle

B-64484EN-1/02 PROGRAMMING

— 85 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

— Front drilling cycle (G83)/side drilling cycle (G87)

T Shown below are the points where a dedicated effective area (for in-position check) is applied in front drilling cycle and side drilling cycle. If no Q (depth of cut for each cutting feed) is specified in a drilling cycle (G83 or G87), an ordinary drilling cycle is assumed.

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

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) 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 levelPoint R

Point Z

M(α+1),P2

Mα

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 In-position width for other than hole bottoms (regular) In-position width for hole bottoms

PROGRAMMING B-64484EN-1/02

— 86 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

— Front high-speed peck drilling cycle (G83, G83.5) / Side high-speed peck drilling cycle (G87, G87.5)

T Shown below are the points where a dedicated effective area (for in-position check) is applied in front high-speed peck drilling cycle and side high-speed peck drilling cycle. In high-speed peck drilling cycles (G83 and G87) (bit 2 (RTR) of parameter No. 5101 = 0), G83.5 and G87.5 can also be used to perform high-speed peck drilling regardless of the setting of the parameter RTR.

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

G87 Z(W)_ C(H)_ X(U)_ R_ P_ Q_ 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 F_ : Cutting feedrate K_ : Number of repeats (When it is needed) 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),P2Point R

Point Z

Initial level

Point R level Point R

Point Z

M(α+1),P2

Mα

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 parameter No. 5114 In-position width for other than hole bottoms (regular) In-position width for other than hole bottoms (for retraction in peck drilling cycle) In-position width for hole bottoms

B-64484EN-1/02 PROGRAMMING

— 87 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

NOTE When setting an effective area (for in-position check) enclosed in , pay

attention to the retraction distance d (parameter No.5114). If the effective area is too large for the retraction distance, it is likely that no retraction may be performed.

— Front peck drilling cycle (G83, G83.6) / Side peck drilling cycle (G87, G87.6)

T Shown below are the points where a dedicated effective area (for in-position check) is applied in front peck drilling cycle and side peck drilling cycle. In peck drilling cycles (G83 and G87) (bit 2 (RTR) of parameter No. 5101 = 1), G83.6 and G87.6 can also be used to perform high-speed peck drilling regardless of the setting of the parameter RTR.

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

G83 or G87 (G98 mode) G83 or G87 (G99 mode)

Point R

Point Z

Initial level

Mα

M(α+1),P2

Point R

Point Z

Point R level

Mα

M(α+1),P2

P1 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 parameter No. 5115 In-position width for other than hole bottoms (regular) In-position width for hole bottoms

PROGRAMMING B-64484EN-1/02

— 88 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

— Front tapping cycle (G84) / Side tapping cycle (G88) T

Shown below are the points where a dedicated effective area (for in-position check) is applied in front tapping cycle and side tapping cycle.

G84 X(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ; or

G88 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) M_ : M code for C-axis clamp (When it is needed.)

G84 or G88 (G98 mode) G84 or G88 (G99 mode)

Point R

Point Z

Spindle CCW

Spindle CW

Initial level

M(α+1),P2

Mα

Point R

Point Z

Spindle CCW

Spindle CW

Point R level

Mα

M(α+1),P2

CAUTION When resuming the initial level, set an effective area (for in-position check)

enclosed in , pay attention to the distance between point R and the workpiece. If the effective area is too large for the distance between point R and the workpiece, it is likely that the workpiece or tool may be damaged, because a rapid traverse may occur before the tool retracts completely from the workpiece.

B-64484EN-1/02 PROGRAMMING

— 89 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

— Front boring cycle (G85) / Side boring cycle (G89) T

Shown below are the points where a dedicated effective area (for in-position check) is applied in front boring cycle and side boring cycle.

G85 X(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ; or

G89 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) M_ : M code for C-axis clamp (When it is needed.)

G85 or G89 (G98 mode) G85 or G89 (G99 mode)

Point R

Point Z

Initial level

M(α+1),P2

Mα

Point R

Point Z

Point R level

Mα

M(α+1),P2

PROGRAMMING B-64484EN-1/02

— 90 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

4.5 RIGID TAPPING Front face tapping cycles (G84) and side face tapping cycles (G88) can be performed either in conventional mode or rigid mode. In conventional mode, the spindle is rotated or stopped, in synchronization with the motion along the tapping axis according to miscellaneous functions M03 (spindle CW rotation), M04 (spindle CCW rotation), and M05 (spindle stop). In rigid mode, the spindle motor is controlled in the same way as a control motor, by the application of compensation to both motion along the tapping axis and that of the spindle. For rigid tapping, each turn of the spindle corresponds to a certain amount of feed (screw lead) along the spindle axis. This also applies to acceleration/deceleration. This means that rigid tapping does not demand the use of float tappers as in the case of conventional tapping, thus enabling high-speed, high-precision tapping. When the system is equipped with the optional multi-spindle control function, the second to fourth spindles can be used for rigid tapping.

4.5.1 FRONT FACE RIGID TAPPING CYCLE (G84) / SIDE FACE RIGID TAPPING CYCLE (G88)

Controlling the spindle motor in the same way as a servo motor in rigid mode enables high-speed tapping. Format

G84 X (U)_ C (H)_ Z (W)_ R_ P_ F_ K_ M_ ;

or G88 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.)

Number of repeats is specified by address L_, in case of bit 1 (FCV) of parameter No.0001 = 1.

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

G84 or G88 (G98 mode) G84 or G88 (G99 mode)

Initial level

Point R

Spindle stopSpindle CW

Point ZP

Point R level

Operation 2 Operation 1 Operation 6

Operation 3

Operation 4

Operation 5

Spindle stop Spindle

Point R

Point Z P

Point R level

Spindle stop Spindle CCW

Spindle stop Spindle stop

Spindle stop

P2 P2Spindle CW

B-64484EN-1/02 PROGRAMMING

— 91 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

P2 performs dwelling of C-axis unclamp. (The dwell time is set in parameter No. 5111.) In front face rigid tapping (G84), the plane first axis is used as the drilling axis and the other axes are used as positioning axes.

Bit 0 (RTX) of parameter No. 5209 Plane selection Drilling axis G17: Xp-Yp plane Xp G18: Zp-Xp plane Zp 0 G19: Yp-Zp plane Yp

1 Zp Xp: X axis or its parallel axis Yp: Y axis or its parallel axis Zp: Z axis or its parallel axis In side face rigid tapping (G88), the plane first axis is used as the drilling axis and the other axes are used as positioning axes.

Bit 0 (RTX) of parameter No. 5209 Plane selection Drilling axis G17: Xp-Yp plane Yp G18: Zp-Xp plane Xp 0 G19: Yp-Zp plane Zp

1 Xp Xp: X axis or its parallel axis Yp: Y axis or its parallel axis Zp: Z axis or its parallel axis

(Series 15 format) G84.2 X (U)_ C (H)_ Z (W)_ R_ P_ F_ L_ S_ ;

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 L_ : Number of repeats (When it is needed.) S_ : Spindle speed C-axis clamp cannot be performed during specification of the Series 15 format.

G84.2 (G98 mode) G84.2 (G99 mode)

Initial level

Point R

Spindle stopSpindle CW

Point ZP

Point R level

Operation 2Operation 1

Operation 6

Operation 3

Operation 4

Operation 5

Spindle stop Spindle

Point R

Spindle CW

Point Z P

Point R level

Spindle stop Spindle CCW

Spindle stop Spindle stop

Spindle stop

PROGRAMMING B-64484EN-1/02

— 92 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

A G code cannot discriminate between front face tapping cycle and side face tapping cycle using Series 15 format commands(G84.2). The drilling axis is determined by plane selection (G17/G18/G19). Specify the plane selection that becomes equivalent to front face tapping cycle or side face tapping cycle as appropriate. (When FXY (bit 0 of parameter No. 5101) is 0, the Z-axis is used as the drilling axis. When FXY is 1, plane selection is as Table 4.5.1 (a).)

Table 4.5.1 (a) Plane selection Drilling axis

G17: Xp-Yp plane Zp G18: Zp-Xp plane Yp G19: Yp-Zp plane Xp

Xp: X axis or its parallel axis Yp: Y axis or its parallel axis Zp: Z axis or its parallel axis Thus, the rigid tapping mode can be specified in two formats: G84/G88(FS16 format) and G84.2(FS15 format). A usable format can be selected by parameter setting.

Parameter Bit 1 (FCV) of

parameter No. 0001 Bit 3 (F16) of

parameter No. 5102 Executable command format

0 — FS16 format only (The number of repeats is specified using address K.)

1 0 FS15 format or FS16 format (The number of repeats is specified using address L.)

1 1 FS16 format only (The number of repeats is specified using address L.)

Explanation Once positioning for the X-axis (G84) or Z-axis (G88) has been completed, the spindle is moved, by rapid traverse, to point R. Tapping is performed from point R to point Z, after which the spindle stops and observes a dwell time. Then, the spindle starts reverse rotation, retracts to point R, stops rotating, then moves to the initial level by rapid traverse. During tapping, the feedrate override and spindle override are assumed to be 100%. For retraction (operation 5), however, a fixed override of up to 2000% can be applied by setting bit 4 (DOV) of parameter No. 5200, bit 3 (OVU) of parameter No. 5201, and parameter No. 5211.

— Rigid mode Rigid mode can be specified by applying any of the following methods: (1) Specifying M29S***** before a tapping block (2) Specifying M29S***** within a tapping block (3) Handling G84 or G88 as a G code for rigid tapping (Set bit 0 (G84) of parameter No. 5200 to 1.)

— Thread lead In feed per minute mode, the feedrate divided by the spindle speed is equal to the thread lead. In feed per rotation mode, the feedrate is equal to the thread lead.

— Series 15 format command Rigid tapping can be performed using Series 15 format commands.

— Acceleration/deceleration after interpolation Linear or bell-shaped acceleration/deceleration can be applied. Details are given later.

— Look-ahead acceleration/deceleration before interpolation Look-ahead acceleration/deceleration before interpolation is invalid.

B-64484EN-1/02 PROGRAMMING

— 93 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

— Override

Various types of override functions are invalid. The following override functions can be enabled by setting corresponding parameters: (1) Extraction override (2) Override signal

— Dry run Dry run can be executed also in G84 (G88). When dry run is executed at the feedrate for the drilling axis in G84 (G88), tapping is performed according to the feedrate. Note that the spindle speed becomes faster at a higher dry run feedrate.

— Machine lock Machine lock can be executed also in G84 (G88). When G84 (G88) is executed in the machine lock state, the tool does not move along the drilling axis. Therefore, the spindle does not also rotate.

— Reset When a reset is performed during rigid tapping, the rigid tapping mode is canceled and the spindle motor enters the normal mode. Note that the G84 (G88) mode is not canceled in this case when bit 6 (CLR) of parameter No. 3402 is set.

— Interlock Interlock can also be applied in G84 (G88).

— Feed hold and single block When bit 6 (FHD) of parameter No. 5200 is set to 0, feed hold and single block are invalid in the G84 (G88) mode. When this bit is set to 1, they are valid.

— Manual feed For rigid tapping by manual handle feed, see the section «Rigid Tapping by Manual Handle.» With other manual operations, rigid tapping cannot be performed.

— Backlash compensation In the rigid tapping mode, backlash compensation is applied to compensate the lost motion when the spindle rotates clockwise or counterclockwise. Set the amount of backlash in parameters Nos. 5321 to 5324. Along the drilling axis, backlash compensation has been applied.

— C-axis clamp, C-axis unclamp It is possible to specify an M code for mechanically fixing or releasing the C-axis during rigid tapping. Adding an M code for clamp to the G84 (G88) block outputs both M codes. Descriptions of timing are provided later. An M code for clamp is set in parameter No. 5110. An M code for unclamp is assumed as Table 4.5.1 (b) depending on the setting of parameter No. 5110.

Table 4.5.1 (b) Parameter No.5110

0 Non-0 No M codes are output. The setting of parameter No.5110 + 1 is assumed.

PROGRAMMING B-64484EN-1/02

— 94 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Limitation — Axis switching

Before the drilling axis can be changed, the canned cycle must be canceled. If the drilling axis is changed in rigid mode, alarm PS0206, “CAN NOT CHANGE PLANE (RIGID TAP)” is issued.

— S commands When a value exceeding the maximum rotation speed for the gear being used is specified, alarm PS0200, “ILLEGAL S CODE COMMAND” is issued. If such a command that the number of pulses of 4 msec or 8 msec is 32768 or more on the detection unit level or the number of pulses of 4 msec or 8 msec is 32768 or more for a serial spindle is specified, alarm PS0202, “POSITION LSI OVERFLOW” is issued. <Example> For a built-in motor equipped with a detector having a resolution of 4095 pulses per rotation, the maximum spindle speed during rigid tapping is as follows (in the case of 8 msec): (4095×1000÷8×60)÷4095=7500 (min-1) For a serial spindle (32767×1000÷8×60)÷4095=60012(min-1) [Note: Ideal value]

— F commands

Specifying a value larger than the upper limit for cutting feed will cause alarm PS0201, “FEEDRATE NOT FOUND IN RIGID TAP” to be issued.

— Unit of F command

Metric input Inch input Remarks G98 1mm/min 0.01inch/min Decimal point programming allowed G99 0.01mm/rev 0.0001inch/rev Decimal point programming allowed

— M29

If an S command and axis movement are specified between M29 and G84, alarm PS0203, “PROGRAM MISS AT RIGID TAPPING” is issued. If M29 is specified in a tapping cycle, alarm PS0204, “ILLEGAL AXIS OPERATION” is issued.

— P Specify P in a block that performs drilling. If P is specified in a non-drilling block, it is not stored as modal data.

— Cancel Do not specify a G code of the 01 group (G00 to G03 or G60 (when the bit 0 (MDL) of parameter No. 5431 is set to 1)) and G84 in a single block. Otherwise, G84 will be canceled.

— Tool offset In the canned cycle mode, tool offsets are ignored.

— Program restart A program cannot be restarted during rigid tapping.

— R The value of R must be specified in a block which performs drilling. If the value is specified in a block which does not perform drilling, it is not stored as modal data.

— Subprogram call In the canned cycle mode, specify the subprogram call command M98P_ in an independent block.

B-64484EN-1/02 PROGRAMMING

— 95 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Example Tapping axis feedrate: 1000 mm/min Spindle speed: 1000 min-1 Screw lead: 1.0 mm <Programming for feed per minute> G98 ; ……………………………….. Command for feed per minute G00 X100.0 ;…………………………… Positioning M29 S1000;…………………………….. Command for specifying rigid mode G84 Z-100.0 R-20.0 F1000 ;……… Rigid tapping <Programming for feed per rotation> G99 ; ……………………………….. Command for feed per rotation G00 X100.0 ;…………………………… Positioning M29 S1000 ;……………………………. Command for specifying rigid mode G84 Z-100.0 R-20.0 F1.0 ;………… Rigid tapping

PROGRAMMING B-64484EN-1/02

— 96 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

4.5.2 Peck Rigid Tapping Cycle (G84 or G88) Tapping a deep hole in rigid tapping mode may be difficult due to chips sticking to the tool or increased cutting resistance. In such cases, the peck rigid tapping cycle is useful. In this cycle, cutting is performed several times until the bottom of the hole is reached. Two peck tapping cycles are available: High-speed peck tapping cycle and standard peck tapping cycle. These cycles are selected using the bit 5 (PCP) of parameter No. 5200.

Format When rigid tapping is specified with G84 (G88) if bit 5 (PCP) of parameter No. 5200 = 0, high-speed peck rigid tapping is assumed.

Point R level

Point Z

Point R

Mα

(1)d (2)

Spindle CCW

Spindle stopM(α+1) P2

Spindle stop Spindle CCW

Spindle stop Spindle CW

Spindle CW

P1 Spindle stop

(3)

Spindle stop

G84 or G88(G98 mode) G84 or G88(G99 mode)

G84 X(U)_ C(H)_Z(W)_ R_ P_ Q_ F_ K_ M_ ;or G88 Z(W)_ C(H)_X(U)_ R_ P_ Q_ 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 the hole Q_ : Depth of cut for each cutting feed F_ : The cutting feedrate K_ : Number of repeats (when it is needed.) M_ : M code for C-axis clamp (when it is needed.)

— High-speed peck rigid tapping cycle In the first cutting from point R, perform cutting by depth «q» specified by address Q while rotating the spindle in the forward direction (operation <1>). Then, perform returning by the amount specified by parameter No. 5213 while rotating the spindle in the reverse direction (operation <2>). Then, perform tapping by (d+q) while rotating the spindle in the forward direction (operation <3>). Repeat operations <2> and <3> until the bottom of the hole is reached. The cutting speed and rigid tapping time constant are used for operations <1> and <3>. For operation <2> and travel from the bottom of the hole (point Z) to point R, rigid tapping extract override is enabled and the rigid tapping extract time constant is used.

d = Amount ofreturn

Spindle stop

(3)

Point R level

P1Spindle stop

Spindle CWPoint R

Point Z

Mα

(1)d(2)

Initial level

Spindle CCW

Spindle stopM(α+1) P2

Spindle stop Spindle CCW

Spindle stopSpindle CW

When rigid tapping is specified with G84 (G88) if bit 5 (PCP) of parameter No. 5200 = 1, peck rigid tapping is assumed.

B-64484EN-1/02 PROGRAMMING

— 97 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

G84 or G88(G98 mode) G84 or G88(G99 mode)

G84 X(U)_ C(H)_Z(W)_ R_ P_ Q_ F_ K_ M_ ;or G88 Z(W)_ C(H)_X(U)_ R_ P_ Q_ F_ K_ M_ ;

d = Cutting start distance

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

— Peck rigid tapping cycle In the first cutting from point R, perform cutting by depth «q» specified by address Q while rotating the spindle in the forward direction (operation <1>). Then, return to point R by rotating the spindle in the reverse direction (operation <2>). Then, rotate the spindle in the forward direction and perform cutting to the position indicated by [(Position to which cutting was performed previously) — (Cutting start distance set in parameter No. 5213)] as movement to the cutting start point (operation <3>). Continue cutting by (d+q) (operation <4>). Repeat operations <2> to <4> until the bottom of the hole is reached. The cutting speed and rigid tapping time constant are used for operations <1> and <4>. For operations <2>, <3>, and travel from the bottom of the hole (point Z) to point R, rigid tapping extract override is enabled and the rigid tapping extract time constant is used.

Spindle stop

Point Z

Mα

(1)d(2)

Initial level

Spindle stopM(α+1) P2 Point R

level

Point R

(3)

(4)

P1Spindle stop

Spindle CW

Spindle CCW

Spindle stop Spindle CCW

Spindle stop Spindle CW

Point Z

Mα

(1)d(2)

Spindle stopM(α+1) P2 Point R

level

Point R

(3)

(4)

Spindle stop

P1 Spindle stop

Spindle CW

Spindle CCW

Spindle stop Spindle CW

Spindle stop Spindle CCW

The symbols in the figure above indicate the following operations.

: Positioning (Rapid traverse G00)

: Cutting feed (Linear interpolation G01) P1 : Dwell programmed by the address P command Mα : Output of the M code for C-axis clamp (The α value is set in parameter No. 5110.)M(α+1) : Output of the M code for C-axis unclamp P2 : Dwell set by parameter No.5111 Note P1, Mα, M(α+1), and P2 are not executed or output without being specified or set.

Explanation — Cutting start distance

Cutting start distance d is set by parameter No. 5213.

— Amount of return Amount of return for each time d is set by parameter No. 5213.

— Return speed For the speed of return operation, a maximum of 2000% of override can be enabled by setting bit 4 (DOV) of parameter No. 5200, bit 3 (OVU) of parameter No. 5201, and parameter No. 5211 as with travel from the bottom of the hole (point Z) to point R.

PROGRAMMING B-64484EN-1/02

— 98 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

— Speed during cutting into the cutting start point For the speed during cutting into the cutting start point, a maximum of 2000% of override can be enabled by setting bit 4 (DOV) of parameter No. 5200, bit 3 (OVU) of parameter No. 5201, and parameter No. 5211 as with travel from the bottom of the hole (point Z) to point R.

— Acceleration/deceleration after interpolation Linear or bell-shaped acceleration/deceleration can be applied.

— Look-ahead acceleration/deceleration before interpolation Look-ahead acceleration/deceleration before interpolation is invalid.

— Override Various types of override functions are invalid. The following override functions can be enabled by setting corresponding parameters: • Extraction override • Override signal Details are given later.

— Interlock Interlock can also be applied in G84 (G88).

— Feed hold and single block When bit 6 (FHD) of parameter No. 5200 is set to 0, feed hold and single block are invalid in the G84 (G88) mode. When this bit is set to 1, they are valid.

— Manual feed For rigid tapping by manual handle feed, see the section «Rigid Tapping by Manual Handle.» With other manual operations, rigid tapping cannot be performed.

— Series 15 format When bit 1 (FCV) of parameter No. 0001 is set to 1, execution is enabled with G84.2. The same operation as with G84 is performed. However, the command format for the repetitive count is L.

B-64484EN-1/02 PROGRAMMING

— 99 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Limitation

— Axis switching Before the drilling axis can be changed, the canned cycle must be canceled. If the drilling axis is changed in rigid mode, alarm PS0206, “CAN NOT CHANGE PLANE (RIGID TAP)” is issued.

— S commands • If a speed higher than the maximum speed for the gear being used is specified, alarm PS0200,

“ILLEGAL S CODE COMMAND” is issued. • When the rigid tapping canned cycle is cancelled, the S command used for rigid tapping is cleared to

S0.

— Distribution amount for the spindle The maximum distribution amount is as follows (displayed on diagnostic data No. 451): • For a serial spindle: 32,767 pulses per 4 msec or 8 msec This amount is changed according to the gear ratio setting for the position coder or rigid tapping

command. If a setting is made to exceed the upper limit, alarm PS0202, “POSITION LSI OVERFLOW” is issued.

— F command

Specifying a value larger than the upper limit for cutting feed will cause alarm PS0011, “FEED ZERO ( COMMAND )” to be issued.

— Unit of F command Metric input Inch input Remarks

G98 1mm/min 0.01inch/min Decimal point programming allowed G99 0.01mm/rev 0.0001inch/rev Decimal point programming allowed

— M29

If an S command and axis movement are specified between M29 and G84, alarm PS0203 is issued. If M29 is specified in a tapping cycle, alarm PS0204 is issued.

— P/Q Specify P and Q in a block that performs drilling. If they are specified in a block that does not perform drilling, they are not stored as modal data. When Q0 is specified, the peck rigid tapping cycle is not performed.

— Cancel Do not specify a G code of the 01 group (G00 to G03 or G60 (when the bit 0 (MDL) of parameter No. 5431 is set to 1)) and G84 in a single block. Otherwise, G84 will be canceled.

— Tool offset In the canned cycle mode, tool offsets are ignored.

— Subprogram call In the canned cycle mode, specify the subprogram call command M98P_ in an independent block.

— Amount of return and cutting start distance Set the amount of return and cutting start distance (parameter No. 5213) so that the tool does not overshoot point R.

PROGRAMMING B-64484EN-1/02

— 100 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

4.5.3 Canned Cycle Cancel (G80) The rigid tapping canned cycle is canceled. For how to cancel this cycle, see II-4.3.4.

NOTE When the rigid tapping canned cycle is cancelled, the S value used for rigid

tapping is also cleared (as if S0 is specified). Accordingly, the S command specified for rigid tapping cannot be used in a

subsequent part of the program after the cancellation of the rigid tapping canned cycle.

After canceling the rigid tapping canned cycle, specify a new S command as required.

4.5.4 Override during Rigid Tapping Various types of override functions are invalid. The following override functions can be enabled by setting corresponding parameters: • Extraction override • Override signal

4.5.4.1 Extraction override For extraction override, the fixed override set in the parameter or override specified in a program can be enabled at extraction (including retraction during peck drilling/high-speed peck drilling).

Explanation — Specifying the override in the parameter

Set bit 4 (DOV) of parameter No. 5200 to 1 and set the override in parameter No. 5211. An override from 0% to 200% in 1% steps can be set. Bit 3 (OVU) of parameter No. 5201 can be set to 1 to set an override from 0% to 2000% in 10% steps.

— Specifying the override in a program Set bit 4 (DOV) of parameter No. 5200 and bit 4 (OV3) of parameter No. 5201 to 1. The spindle speed at extraction can be specified in the program. Specify the spindle speed at extraction using address «J» in the block in which rigid tapping is specified. Example) To specify 1000 min-1 for S at cutting and 2000 min-1 for S at extraction . M29 S1000 ; G84 Z-100.0 F1000.0 J2000 ; . The difference in the spindle speed is converted to the actual override by the following calculation. Therefore, the spindle speed at extraction may not be the same as that specified at address «J». If the override does not fall in the range between 100% and 200%, it is assumed to be 100%.

100S

J×=

) at (specified speed Spindle

) at (specified extraction at speed Spindle %)( Override

The override to be applied is determined according to the setting of parameters and that in the command as shown in the Table 4.5.4.1 (a).

B-64484EN-1/02 PROGRAMMING

— 101 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Table 4.5.4.1 (a) DOV = 1 Parameter setting

Command OV3 = 1 OV3 = 0 DOV = 0

Within the range between 100% to 200%

Command in the program Spindle speed at extraction

specified at address «J» Outside the range between 100% to 200%

100%

No spindle speed at extraction specified at address «J» Parameter No. 5211

Parameter No. 5211

100%

NOTE 1 Do not use a decimal point in the value specified at address «J». If a decimal point is used, the value is assumed as follows:

Example) When the increment system for the reference axis is IS-B

• When pocket calculator type decimal point programming is not used The specified value is converted to the value for which the least input

increment is considered. «J200.» is assumed to be 200000 min-1. • When pocket calculator type decimal point programming is used The specified value is converted to the value obtained by rounding down

to an integer. «J200.» is assumed to be 200 min-1.

2 Do not use a minus sign in the value specified at address «J». If a minus sign is used, a value outside the range between 100% to 200% is

assumed. 3 The maximum override is obtained using the following equation so that the

spindle speed to which override at extraction is applied do not exceed the maximum used gear speed (specified in parameters Nos. 5241 to 5244). For this reason, the obtained value is not the same as the maximum spindle speed depending on the override.

100S

×=) at (specified speed Spindle

)parameters in (specified speed spindle Maximum(%) override Maximum

4 When a value is specified at address «J» for specifying the spindle speed at extraction in the rigid tapping mode, it is valid until the canned cycle is canceled.

4.5.4.2 Override signal

By setting bit 4 (OVS) of parameter No. 5203 to 1, override can be applied to cutting/extraction operation during rigid tapping as follows: (1) Applying override using the feedrate override signal (When the second feedrate override signal is enabled, the second feedrate override is applied to the

feedrate to which feedrate override is applied.) (2) Canceling override using the override cancel signal There are the following relationships between this function and override to each operation: (1) At cutting When the override cancel signal is set to 0: Value specified by the override signal When the override cancel signal is set to 1: 100% (3) At extraction

— When the override cancel signal is set to 0: Value specified by the override signal — When the override cancel signal is set to 1 and extraction override is disabled: 100%

PROGRAMMING B-64484EN-1/02

— 102 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

— When the override cancel signal is set to 1 and extraction override is enabled: Value specified for extraction override

NOTE 1 The maximum override is obtained using the following equation so that the

spindle speed to which override is applied do not exceed the maximum used gear speed (specified in parameters Nos. 5241 to 5244). For this reason, the obtained value is not the same as the maximum spindle speed depending on the override.

100S

×=) at (specified speed Spindle

)parameters in (specified speed spindle Maximum(%) override Maximum

2 Since override operation differs depending on the machine in use, refer to the manual provided by the machine tool builder.

B-64484EN-1/02 PROGRAMMING

— 103 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

4.6 CANNED GRINDING CYCLE (FOR GRINDING MACHINE) With the canned grinding cycle, repetitive machining operations that are specific to grinding and are usually specified using several blocks can be specified using one block including a G function. So, a program can be created simply. At the same time, the size of a program can be reduced, and the memory can be used more efficiently. Four types of canned grinding cycles are available: • Traverse grinding cycle (G71) (G72 when G code system C is used) • Traverse direct constant-size grinding cycle (G72) (G73 when G code system C is used) • Oscillation grinding cycle (G73) (G74 when G code system C is used) • Oscillation direct constant-size grinding cycle (G74) (G75 when G code system C is used) In the descriptions below, an axis used for cutting with a grinding wheel and an axis used for grinding with a grinding wheel are referred to as follows: Axis used for cutting with a grinding wheel: Cutting axis Axis used for grinding with a grinding wheel: Grinding axis During execution of a canned grinding cycle, the following functions cannot be used: • Programmable mirror image • Scaling • Coordinate system rotation • 3-dimensional coordinate conversion • One-digit F code feed • Tool length compensation For a depth of cut on a cutting axis and a distance of grinding on a grinding axis, the incremental system (parameter No. 1013) for the reference axis (parameter No. 1031) is used. If 0 is set in parameter No. 1031 (reference axis), the incremental system for the first axis is used.

WARNING The G codes for canned grinding cycles G71, G72, G73, and G74 (G72, G73,

G74, and G75 when G code system C is used) are G codes of group 01. A G code for cancellation such as G80 used for a canned cycle for drilling is unavailable. By specifying a G code of group 00 other than G04, modal information such as a depth of cut is cleared but no canned grinding cycle can be canceled. To cancel a canned grinding cycle, a G code of group 01 other than G71, G72, G73, and G74 needs to be specified. So, when switching to another axis move command from G71, G72, G73 or G74, for example, be sure to specify a G code of group 01 such as G00 or G01 to cancel the canned grinding cycle. If another axis move command is specified without canceling the canned grinding cycle, an unpredictable operation can result because of continued cycle operation.

PROGRAMMING B-64484EN-1/02

— 104 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

NOTE 1 If the G code for a canned grinding cycle (G71, G72, G73, or G74) is specified,

the canned grinding cycle is executed according to the values of A, B, W, U, I, and K preserved as modal data while the cycle is valid, even if a block specified later specifies none of G71, G72, G73, and G74.

Example: G71 A_ B_ W_ U_ I_ K_ H_ ;

; ← The canned grinding cycle is executed even if an empty block is specified. %

2 When switching from a canned cycle for drilling to a canned grinding cycle, specify G80 to cancel the canned cycle for drilling.

3 When switching from a canned grinding cycle to another axis move command, cancel the canned cycle according to the warning above.

4 A canned grinding cycle and multiple repetitive canned cycle cannot be used simultaneously on the same path.

If both options are specified, which function to use can be selected with bit 0 (GFX) of parameter No. 5106.

B-64484EN-1/02 PROGRAMMING

— 105 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

4.6.1 Traverse Grinding Cycle (G71) A traverse grinding cycle can be executed.

Format G71 A_ B_ W_ U_ I_ K_ H_ ;

A_ : First depth of cut (The cutting direction depends on the sign.) B_ : Second depth of cut (The cutting direction depends on the sign.) W_ : Grinding range (The grinding direction depends on the sign.) U_ : Dwell time I_ : Feedrate for A and B K_ : Feedrate for W H_ : Repetitive count (from 1 to 9999)

G71

<1>(I)

<2>U

<3>(K)

<4>(I)

<5>U<6>(K)

Explanation The traverse grinding cycle consists of six operations. The operations from <1> to <6> are repeated until the repetitive count specified in address H is reached. In the case of single block operation, the operations from <1> to <6> are executed with one cycle start operation.

— Operation sequence in a cycle <1> Cutting with a grinding wheel

By the first depth of cut specified in A, cutting is performed by cutting feed in the X-axis direction. The feedrate specified in I is used.

<2> Dwell A dwell operation is performed for the time specified in U.

<3> Grinding A movement is made by the distance specified in W by cutting feed. Set a grinding axis in

parameter No.5176. The feedrate specified in K is used. <4> Cutting with a grinding wheel

By the second depth of cut specified in B, cutting is performed by cutting feed in the X-axis direction. The feedrate specified in I is used.

<5> Dwell A dwell operation is performed for the time specified in U.

<6> Grinding (return direction) A movement is made at the feedrate specified in K in the reverse direction by the distance

specified in W.

PROGRAMMING B-64484EN-1/02

— 106 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Limitation — Cutting axis

As a cutting axis, the first controlled axis is used. By setting bit 0 (FXY) of parameter No. 5101 to 1, the axis can be switched using a plane selection command (G17, G18, or G19).

— Grinding axis Specify a grinding axis by setting an axis number for other than the cutting axis in parameter No. 5176. Specify a grinding command in W at all times without using an axis name. The axis name corresponding to the set axis number can also be used for specification.

— A, B, W The commands of A, B, and W are all incremental commands. When none of A and B are specified or A=B=0, spark-out operation (execution of only movement in the grinding direction) is performed.

— H When H is not specified or H=0, the specification of H=1 is assumed. The specification of H is valid only in the block where H is specified.

— Clear The data A, B, W, U, I, and K in the canned cycle is modal information common to G71, G72, G73, and G74. So, the data remains valid until new data is specified. The data is cleared when a G code of group 00 other than G04 or a G code of group 01 other than G71, G72, G73, and G74 is specified. The specification of H is valid only in the block where H is specified.

— B code During the canned cycle, no B code (second auxiliary function) can be specified.

NOTE 1 If no grinding axis is specified when G71 is specified, alarm PS0455, “ILLEGAL

COMMAND IN GRINDING” is issued. 2 If the specified cutting axis number and grinding axis number are the same,

alarm PS0456, “ILLEGAL PARAMETER IN GRINDING” is issued. 3 Even if G90 (absolute command) is specified while this cycle is valid, each of the

A, B, and W commands is an incremental command.

B-64484EN-1/02 PROGRAMMING

— 107 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

4.6.2 Traverse Direct Constant-Size Grinding Cycle (G72) A traverse direct constant-size grinding cycle can be executed.

Format G72 P_ A_ B_ W_ U_ I_ K_ H_ ;

P_ : Gage number (1 to 4) A_ : First depth of cut (The cutting direction depends on the sign.) B_ : Second depth of cut (The cutting direction depends on the sign.) W_ : Grinding range (The grinding direction depends on the sign.) U_ : Dwell time I_ : Feedrate for A and B K_ : Feedrate for W H_ : Repetitive count (from 1 to 9999)

G72

<1>(I)

<2>U

<3>(K)

<4>(I)

<5>U<6>(K)

Explanation If the multi-step skip option is specified, a gage number can be specified. The method of gage number specification is the same as for the multi-step skip option. If the multi-step skip option is not specified, the conventional skip signal is used. The commands and operations other than gage number specification are the same as for G71.

— Operation performed when the skip signal is input A G72 cycle can be terminated after interrupting the current operation (or after ending the current operation) by inputting the skip signal during execution of the cycle. Each operation of the sequence performed when the skip signal is input is described below. • If the skip signal is input during operation <1> or <4> (movement by A or B), cutting is immediately

stopped to return to coordinate α selected as the cycle start point.

(End)

Skip signal

(End)

• If the skip signal is input during operation <2> or <5> (dwell), dwell operation is immediately stopped to return to coordinate α selected as the cycle start point.

PROGRAMMING B-64484EN-1/02

— 108 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

• If the skip signal is input during operation <3> or <6> (grinding feed), the tool returns to coordinate α selected as the cycle start point after the end of movement over W.

(End)

Skip signal

Skip signal (End)

Limitation

— Cutting axis As a cutting axis, the first controlled axis is used. By setting bit 0 (FXY) of parameter No. 5101 to 1, the axis can be switched using a plane selection command (G17, G18, or G19).

— Grinding axis Specify a grinding axis by setting an axis number for other than the cutting axis in parameter No. 5177. Specify a grinding command in W at all times without using an axis name. The axis name corresponding to the set axis number can also be used for specification.

— P If a value other than P1 to P4 is specified, the skip function is disabled. The specification of P is valid only in the block where P is specified.

— H When H is not specified or H=0, the specification of H=1 is assumed. The specification of H is valid only in the block where H is specified.

— B code During the canned cycle, no B code (second auxiliary function) can be specified.

NOTE 1 If no grinding axis is specified when G72 is specified, alarm PS0455, “ILLEGAL

COMMAND IN GRINDING” is issued. 2 If the specified cutting axis number and grinding axis number are the same,

alarm PS0456, “ILLEGAL PARAMETER IN GRINDING” is issued. 3 Even if G90 (absolute command) is specified while this cycle is valid, each of the

A, B, and W commands is an incremental command.

B-64484EN-1/02 PROGRAMMING

— 109 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

NOTE 4 If a value from P1 to P4 is specified without specifying the multi-step skip option,

alarm PS0370, “G31P/G04Q ERROR” is issued.

4.6.3 Oscillation Grinding Cycle (G73) An oscillation grinding cycle can be executed.

Format G73 A_ (B_) W_ U_ K_ H_ ;

A_ : First depth of cut (The cutting direction depends on the sign.) B_ : Second depth of cut (The cutting direction depends on the sign.) W_ : Grinding range (The grinding direction depends on the sign.) U_ : Dwell time K_ : Feedrate for W H_ : Repetitive count (from 1 to 9999)

G73

A(B)

<1>U<2>(K)

<3>U<4>(K)

Explanation The oscillation grinding cycle consists of four operations. The operations from <1> to <4> are repeated until the repetitive count specified in address H is reached. In the case of single block operation, the operations from <1> to <4> are executed with one cycle start operation.

— Operation sequence in a cycle <1> Dwell

A dwell operation is performed for the time specified in U. <2> Cutting + grinding with a grinding wheel

Cutting feed is performed on the cutting axis (X-axis) and a grinding axis at the same time. The amount of movement on the cutting axis (depth of cut) is the first depth of cut specified in A, and the amount of movement on a grinding axis is the distance specified in W. Set a grinding axis in parameter No.5178. The feedrate specified in K is used.

<3> Dwell A dwell operation is performed for the time specified in U.

<4> Cutting + grinding with a grinding wheel (return direction) Cutting feed is performed on the cutting axis (X-axis) and a grinding axis at the same time. The

amount of movement on the cutting axis (depth of cut) is the second depth of cut specified in B, and the amount of movement on the grinding axis is the distance specified in W. The feedrate specified in K is used.

PROGRAMMING B-64484EN-1/02

— 110 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Limitation — Cutting axis

As a cutting axis, the first controlled axis is used. By setting bit 0 (FXY) of parameter No. 5101 to 1, the axis can be switched using a plane selection command (G17, G18, or G19).

— Grinding axis Specify a grinding axis by setting an axis number for other than the cutting axis in parameter No. 5178. Specify a grinding command in W at all times without using an axis name. The axis name corresponding to the set axis number can also be used for specification.

— B If B is not specified, B=A is assumed. The specification of B is valid only in the block where B is specified.

— H When H is not specified or H=0, the specification of H=1 is assumed. The specification of H is valid only in the block where H is specified.

— Clear The data A, W, U, and K in the canned cycle is modal information common to G71, G72, G73, and G74. So, the data remains valid until new data is specified. The data is cleared when a G code of group 00 other than G04 or a G code of group 01 other than G71, G72, G73, and G74 is specified. The specification of B or H is valid only in the block where B or H is specified.

— B code During the canned cycle, no B code (second auxiliary function) can be specified.

NOTE 1 If no grinding axis is specified when G73 is specified, alarm PS0455, “ILLEGAL

COMMAND IN GRINDING” is issued. 2 If the specified cutting axis number and grinding axis number are the same,

alarm PS0456, “ILLEGAL PARAMETER IN GRINDING” is issued. 3 Even if G90 (absolute command) is specified while this cycle is valid, each of the

A, B, and W commands is an incremental command.

B-64484EN-1/02 PROGRAMMING

— 111 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

4.6.4 Oscillation Direct Constant-Size Grinding Cycle (G74) An oscillation direct constant-size grinding cycle can be executed.

Format G74 P_ A_ (B_) W_ U_ K_ H_ ;

P_ : Gage number (1 to 4) A_ : First depth of cut (The cutting direction depends on the sign.) B_ : Second depth of cut (The cutting direction depends on the sign.) W_ : Grinding range (The grinding direction depends on the sign.) U_ : Dwell time K_ : Feedrate for W H_ : Repetitive count (from 1 to 9999)

G74

A(B)

<1>U<2>(K)

<3>U<4>(K)

— Operation performed when the skip signal is input A G74 cycle can be terminated after interrupting the current operation (or after ending the current operation) by inputting the skip signal during execution of the cycle. Each operation of the sequence performed when the skip signal is input is described below. • If the skip signal is input during operation <1> or <3> (dwell), dwell operation is immediately

stopped to return to coordinate α selected as the cycle start point. • If the skip signal is input during operation <2> or <4> (A, B, grinding feed), the tool returns to

coordinate α selected as the cycle start point after the end of movement over W.

(End)

Skip signal

(End)

Skip signal

PROGRAMMING B-64484EN-1/02

— 112 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Limitation — Cutting axis

As a cutting axis, the first controlled axis is used. By setting bit 0 (FXY) of parameter No. 5101 to 1, the axis can be switched using a plane selection command (G17, G18, or G19).

— Grinding axis Specify a grinding axis by setting an axis number for other than the cutting axis in parameter No. 5179. Specify a grinding command in W at all times without using an axis name. The axis name corresponding to the set axis number can also be used for specification.

— P If a value other than P1 to P4 is specified, the skip function is disabled. The specification of P is valid only in the block where P is specified.

— B If B is not specified, B=A is assumed. The specification of B is valid only in the block where B is specified.

— H When H is not specified or H=0, the specification of H=1 is assumed. The specification of H is valid only in the block where H is specified.

— Clear The data A, W, U, and K in the canned cycle is modal information common to G71, G72, G73, and G74. So, the data remains valid until new data is specified. The data is cleared when a G code of group 00 other than G04 or a G code of group 01 other than G71, G72, G73, and G74 is specified. The specification of P, B, or H is valid only in the block where P, B, or H is specified.

— B code During the canned cycle, no B code (second auxiliary function) can be specified.

NOTE 1 If no grinding axis is specified when G74 is specified, alarm PS0455, “ILLEGAL

COMMAND IN GRINDING” is issued. 2 If the specified cutting axis number and grinding axis number are the same,

alarm PS0456, “ILLEGAL PARAMETER IN GRINDING” is issued. 3 Even if G90 (absolute command) is specified while this cycle is valid, each of the

A, B, and W commands is an incremental command. 4 If a value from P1 to P4 is specified without specifying the multi-step skip option,

alarm PS0370, “G31P/G04Q ERROR” is issued.

B-64484EN-1/02 PROGRAMMING

— 113 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

4.7 CHAMFERING AND CORNER R

Overview A chamfering or corner R block can automatically be inserted between linear interpolation (G01) along a single axis and that along a single axis normal to that single axis. Chamfering or corner R is inserted for a command to move the tool along two axes on the plane determined by the plane selection (G17, G18, or G19) command.

Format — Chamfering First axis on the selected plane → second axis on the selected plane (G17 plane: XP → YP, G18 plane: ZP → XP, G19 plane: YP → ZP)

Format G17 plane: G01 XP(U)_ J(C)±j ; G18 plane: G01 ZP(W)_ I(C)±i ; G19 plane: G01 YP(V)_ K(C)±k ;

Explanation Tool movement XP(U)__ YP(V)__ ZP(W)__

Specifies movement from point a to point b with an absolute or incremental programming in the figure on the right. XP is the address of the X-axis of the three basic axes or an axis parallel to the X-axis. YP is the address of the Y-axis of the three basic axes or an axis parallel to the Y-axis. ZP is the address of the Z-axis of the three basic axes or an axis parallel to the Z-axis.

I(C)±i J(C)±j K(C)±k

Specify the distance between points b and c in the figure shown at right with a sign following address I, J, K, or C. (Use I, J, or K when bit 4 (CCR) of parameter No. 3405 is set to 0 or C when the bit is set to 1.)

a d

i, j, k

45° 45°

Positive direction alongthe second axis on theselected plane

Negative directionalong the second axison the selected plane

Start point

Moves from a to d and c. (Positive direction along the second axis on the selected plane when a plus sign is specified at I, J, K, or C or negative direction when a minus sign is specified at I, J, K, or C)

PROGRAMMING B-64484EN-1/02

— 114 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

— Chamfering Second axis on the selected plane → first axis on the selected plane (G17 plane: YP → XP, G18 plane: XP → ZP, G19 plane: ZP → YP)

Format G17 plane: G01 YP(V)_ I(C)±i ; G18 plane: G01 XP(U)_ K(C)±k ; G19 plane: G01 ZP(W)_ J(C)±j ;

Explanation Tool movement XP(U)__ YP(V)__ ZP(W)__

I(C)±i J(C)±j K(C)±k

Moves from a to d and c. (Positive direction along the first axis on the selected plane when a plus sign is specified at I, J, K, or C or negative direction when a minus sign is specified at I, J, K, or C)

c c b i, j, k i, j, k

45°

First axis on the selected plane

45°

First axis onthe selectedplane

Start point

— Corner R First axis on the selected plane → second axis on the selected plane (G17 plane: XP → YP, G18 plane: ZP → XP, G19 plane: YP → ZP)

Format G17 plane: G01 XP(U)_ R±r ; G18 plane: G01 ZP(W)_ R±r ; G19 plane: G01 YP(V)_ R±r ;

Explanation Tool movement XP(U)__ YP(V)__ ZP(W)__

R±r

Specify the radius of the arc connecting points d and c in the figure shown at right with a sign following address R.

a d

Positive direction alongthe second axis on theselected plane

Negative direction alongthe second axis on theselected plane

Start point

Moves from a to d and c. (Positive direction along the second axis on the selected plane when +r is specified at R or negative direction when -r is specified at R)

B-64484EN-1/02 PROGRAMMING

— 115 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

— Corner R Second axis on the selected plane → first axis on the selected plane (G17 plane: YP → XP, G18 plane: XP → ZP, G19 plane: ZP → YP)

Format G17 plane: G01 YP(V)_ R±r ; G18 plane: G01 XP(U)_ R±r ; G19 plane: G01 ZP(W)_ R±r ;

Explanation Tool movement XP(U)__ YP(V)__ ZP(W)__

R±r

Specify the radius of the arc connecting points d and c in the figure shown at right with a sign following address R.

Moves from a to d and c. (Positive direction along the first axis on the selected plane when +r is specified at R or negative direction when -r is specified at R)

c c b

r r

First axis onthe selectedplane

a Start point

Explanation By G01 specified for chamfering or corner R, the tool must be moved only along one of the two axes on the selected plane. The command in the next block must move the tool only along the other axis on the selected plane. Example: When the A-axis is set as an axis parallel to the basic X-axis (by setting parameter No. 1022 to 5),

the following program performs chamfering between cutting feed along the A-axis and that along the Z-axis: G18 A0 Z0 G00 A100.0 Z100.0 G01 A200.0 F100 K30.0 Z200.0

The following program causes an alarm. (Because chamfering is specified in the block to move the tool along the X-axis, which is not on the selected plane) G18 A0 Z0 G00 A100.0 Z100.0 G01 X200.0 F100 K30.0 Z200.0

The following program also causes an alarm. (Because the block next to the chamfering command moves the tool along the X-axis, which is not on the selected plane) G18 A0 Z0 G00 A100.0 Z100.0 G01 Z200.0 F100 I30.0 X200.0

A radius value is specified at I, J, K, R, and C. In an incremental programming, use point b in the figure in «Format» as the start point in the block next to a chamfering or corner R block. That is, specify the distance from point b. Do not specify the distance from point c.

PROGRAMMING B-64484EN-1/02

— 116 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Example

270.0

K3.0

Cutting start point

End point

530.0

φ860

φ268

N003

N004

N002R6

N001 G18 ;N002 G00 X268.0 Z530.0 ;N003 G01 Z270.0 R6.0 ;N004 X860.0 K-3.0 ;N005 Z0 ;

Limitation — Alarms

In the following cases, an alarm is issued:

1) Chamfering or corner R is specified in a block for threading (alarm PS0050, “CHF/CNR NOT ALLOWED IN THRD BLK”).

2) G01 is not specified in the block next to the G01 block in which chamfering or corner R is specified (alarm PS0051, “MISSING MOVE AFTER CNR/CHF” or PS0052, “CODE IS NOT G01 AFTER CHF/CNR”).

3) An axis which is not on the selected plane is specified as a move axis in the block in which chamfering or corner R is specified or the next block (alarm PS0051 or PS0052).

4) A plane selection command (G17, G18, or G19) is specified in the block next to the block in which chamfering or corner R is specified (alarm PS0051).

5) When bit 4 (CCR) of parameter No. 3405 is set to 0 (to specify chamfering at I, J, or K), two or more of I, J, K, and R are specified in G01 (alarm PS0053, “TOO MANY ADDRESS COMMANDS”).

6) Chamfering or corner R is specified in the G01 block to move the tool along more than one axis (alarm PS0054, “NO TAPER ALLOWED AFTER CHF/CNR”).

7) The travel distance along an axis specified in the block in which chamfering or corner R is specified is smaller than the amount of chamfering or corner R (alarm PS0055, “MISSING MOVE VALUE IN CHF/CNR”). (See the Fig. 4.7 (a).)

The solid line indicatesthe tool path whenchamfering is notperformed.

50.0

G18 G01 W30.0 F100.0 I50.0 ; G01 U100.0 ;

Chamfering block tobe inserted

50.0

30.0 (smaller than 50.0)

Fig. 4.7 (a) Example of machining which causes alarm PS0055

B-64484EN-1/02 PROGRAMMING

— 117 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

An invalid combination of a move axis and I, J, or K is specified for chamfering (alarm PS0306, “MISMATCH AXIS WITH CNR/CHF”).

9) An invalid sign is specified at I, J, K, R, or C (chamfering or corner R in the direction opposite to the movement in the next block is specified) (alarm PS0051). (See the Fig. 4.7 (b).)

The solid line indicates thetool path when chamferingis not performed.(negative X direction)

G18 G01 W100.0 F100.0 I50.0 ; G01 U-100.0 ;

Chamfering block tobe inserted (positive Xdirection)

Fig. 4.7 (b) Example of machining which causes alarm PS0051

— Single block operation

When the block in which chamfering or corner R is specified is executed in the single block mode, operation continues to the end point of the inserted chamfering or corner R block and the machine stops in the feed hold mode at the end point. When bit 0 (SBC) of parameter No. 5105 is set to 1, the machine stops in the feed hold mode also at the start point of the inserted chamfering or corner R block.

— Cutter compensation or tool nose radius compensation When applying cutter or tool nose radius compensation, note the following points: 1. If the amount of inner chamfering or corner R is too small as compared with compensation and

cutting is generated, alarm PS0041, “INTERFERENCE IN CUTTER COMPENSATION” is issued. (See the Fig. 4.7 (c).)

Example of machining which does notcause alarm PS0041

Example of machining whichcauses alarm PS0041

(The solid line indicates the programmed path after chamfering. Thedotted line indicates the tool center path or tool nose radius center path.)

Fig. 4.7 (c) 2. A function is available which intentionally changes the compensation direction by specifying the I, J,

or K command in the G01 block in the cutter or tool nose radius compensation mode (see the explanations of cutter or tool nose radius compensation). To use this function when the chamfering and corner R function is used, set bit 4 (CCR) of parameter No. 3405 to 1 so that I, J, and K are not used for specifying chamfering. Operation to be performed under each condition is explained below. (1) When the chamfering and corner R function is not used In the G01 block in the cutter or tool nose radius compensation mode, the cutter or tool nose

radius compensation direction can be specified at address I, J, or K. No chamfering is performed.

PROGRAMMING B-64484EN-1/02

— 118 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

(2) When the chamfering and corner R function is used (2-1) When bit 4 (CCR) of parameter No. 3405 is set to 0 In the G01 block in the cutter or tool nose radius compensation mode, chamfering can be

specified at address I, J, or K. Corner R can also be specified at address R. The cutter or tool nose radius compensation direction cannot be specified. (2-2) When bit 4 (CCR) of parameter No. 3405 is set to 1 In the G01 block in the cutter or tool nose radius compensation mode, the cutter or tool

nose radius compensation direction can be specified at address I, J, or K. Chamfering or corner R can also be specified at address C or R.

B-64484EN-1/02 PROGRAMMING

— 119 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

4.8 MIRROR IMAGE FOR DOUBLE TURRET (G68, G69)

Overview When a unit has a double turret consisting of two tool posts which face each other on the same controlled axis, mirror image can be applied to the X-axis with a G code command. Symmetrical cutting can be performed by creating a machining program for the facing tool posts as if they were in the coordinate system on the same side.

Format

G68 : Double turret mirror image on G69 : Mirror image cancel

Explanation

Mirror image can be applied to the X-axis of the three basic axes that is set by parameter No. 1022 with the G code command. When G68 is designated, the coordinate system is shifted to the double turret side, and the X-axis sign is reversed from the programmed command to perform symmetrical cutting. This function is called the mirror image for double turret. To use this function, set the distance between the two tool posts to a parameter No. 1290.

Example

• For turning

Offset value of toolpost B

Tool post B

120

180

φ120

φ80 φ40

<1>

<2>

Offset value of toolpost A

Tool post A<3>

X40.0 Z180.0 T0101 ; Position tool post A at <1> G68 ; Shift the coordinate system by the distance A to B (120mm), and turn mirror

image on. X80.0 Z120.0 T0202 ; Position tool post B at <2> G69 ; Shift the coordinate system by the distance B to A, and cancel mirror image. X120.0 Z60.0 T0101 ; Position tool post A at <3>

PROGRAMMING B-64484EN-1/02

— 120 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

NOTE A diameter value is specified for the X-axis.

Limitation

NOTE 1 When the G68 command based on this function is enabled, the X-axis

coordinate value that can be read with the custom macro system variables #5041 and up or #100101 and up (current specified position (in the workpiece coordinate system)) is a position with mirror image applied.

2 This function cannot be used together with the balance cut function. If both optional functions are specified, the operation depends on the combination of the systems as follows:

System in which this function is used • One-path system • One-path and loader-path system

System in which this function does not operate • System with two or more paths

4.9 DIRECT DRAWING DIMENSION PROGRAMMING

Overview Angles of straight lines, chamfering value, corner R values, and other dimensional values on machining drawings can be programmed by directly inputting these values. In addition, the chamfering and corner R can be inserted between straight lines having an optional angle. This programming is only valid in memory operation mode.

Format Examples of command formats for the G18 plane (ZX plane) are shown. This function can be specified in the following formats also for the G17 plane (XY plane) and G19 plane (YZ plane). The following formats are changed as follows: For the G17 plane: Z → X, X → Y For the G19 plane: Z → Y, X → Z

Table 4.9 (a) Commands table Commands Movement of tool

1 X2_ (Z2_), A_ ;

(X1 , Z1)

(X2 , Z2)

B-64484EN-1/02 PROGRAMMING

— 121 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Commands Movement of tool

2 ,A1_ ; X3_ Z3_, A2_ ;

(X1 , Z1)

(X3 , Z3)

(X2 , Z2)

X2_ Z2_, R1_ ; X3_ Z3_ ; or ,A1_, R1_ ; X3_ Z3_, A2_ ;

(X1 , Z1)

(X3 , Z3)

(X2 , Z2)

A2 R1

X2_ Z2_, C1_ ; X3_ Z3_ ; or ,A1_, C1_ ; X3_ Z3_, A2_ ;

(X1 , Z1)

(X3 , Z3)

(X2 , Z2)

X2_ Z2_ , R1_ ; X3_ Z3_ , R2_ ; X4_ Z4_ ; or ,A1_, R1_ ; X3_ Z3_, A2_, R2_ ; X4_ Z4_ ;

(X1 , Z1)

(X3 , Z3)(X4 , Z4)

(X2 , Z2)

X2_ Z2_ , C1_ ; X3_ Z3_ , C2_ ; X4_ Z4_ ; or ,A1_, R1_ ; X3_ Z3_, A2_, C2_ ; X4_ Z4_ ;

(X1 , Z1)

(X3 , Z3)

(X2 , Z2)

(X4 , Z4)

PROGRAMMING B-64484EN-1/02

— 122 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

Commands Movement of tool

X2_ Z2_ , R1_ ; X3_ Z3_ , C2_ ; X4_ Z4_ ; or ,A1_, R1_ ; X3_ Z3_, A2_, C2_ ; X4_ Z4_ ;

(X1 , Z1)

(X3 , Z3)

(X2 , Z2)

A2(X4 , Z4)

A1R1

X2_ Z2_ , C1_ ; X3_ Z3_ , R2_ ; X4_ Z4_ ; or ,A1_, C1_ ; X3_ Z3_, A2_, R2_ ; X4_ Z4_ ;

(X1 , Z1)

(X3 , Z3)

(X2 , Z2)

(X4 , Z4)

Explanation A program for machining along the curve shown in Fig. 4.9 (a) is as follows :

a2,A (a1) , C (c1) ;X (x3) Z (z3) , A (a2) , R (r2) ;X (x4) Z (z4) ;

(x3, z3)

(x4, z4)

(x2, z2)

(x1, z1)Start

X (x2) Z (z2) , C (c1) ;X (x3) Z (z3) , R (r2) ;X (x4) Z (z4) ;

or r2

Fig. 4.9 (a) Machining Drawing (example)

For command a straight line, specify one or two out of X, Z, and A. If only one is specified, the straight line must be primarily defined by a command in the next block. To command the degree of a straight line or the value of chamfering or corner R, command with a comma (,) as follows : ,A_ ,C_ ,R_ By specifying 1 to bit 4 (CCR) of parameter No.3405 on the system which does not use A or C as an axis name, the degree of a straight line or the value of chamfering or corner R can be commanded without a comma (,) as follows : A_ C_ R_

B-64484EN-1/02 PROGRAMMING

— 123 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

— Command using a supplement

When bit 5 (DDP) of parameter No. 3405 is set to 1, an angle can be specified using a supplement. There is the following relationship, assuming that the supplement is A’ and the actual specified angle is A: A = 180 – A’

A’A

Fig. 4.9 (b) Supplement

Limitation

NOTE 1 Direct drawing dimension programming commands are valid only during memory

operation. 2 The following G codes are not applicable to the same block as commanded by

direct input of drawing dimensions or between blocks of direct input of drawing dimensions which define sequential figures. (a) G codes other than G04 in group 00 (b) G codes other than G00, G01, and G33 in group 01 (c) G codes in group 10 (canned cycle for drilling) (d) G codes in group 16 (plane selection) (e) G22 and G23

3 Corner R cannot be inserted into a threading block. 4 When the chamfering and corner R and direct drawing dimension programming

options are available, both functions cannot be used simultaneously. When bit 0 (CRD) of parameter No. 3453 is set to 1, direct drawing dimension programming is enabled. (At this time, chamfering and corner R are disabled.)

5 When the end point of the previous block is determined in the next block according to sequential commands of direct drawing dimension programming during single block operation, the machine does not stop in the single block stop mode, but stop in the feed hold stop mode at the end point of the previous block.

6 The angle allowance in calculating the point of intersection in the program below is ±1°.

(Because the travel distance to be obtained in this calculation is too large.) (a) X_ ,A_ ; (If a value within 0°±1° or 180°±1° is specified for the angle

instruction A, the alarm PS0057, “NO SOLUTION OF BLOCK END” occurs.) (b) Z_ ,A_ ; (If a value within 90°±1° or 270°±1° is specified for the angle

instruction A, the alarm PS0057 occurs.) 7 An alarm PS0058, “END POINT NOT FOUND” occurs if the angle made by the 2

lines is within ±1° when calculating the point of intersection. 8 Chamfering or corner R is ignored if the angle made by the 2 lines is within ±1°.

PROGRAMMING B-64484EN-1/02

— 124 —

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

NOTE 9 Both a dimensional command (absolute programming) and angle instruction

must be specified in the block following a block in which only the angle instruction is specified.

(Example) N1 X_ ,A_ ,R_ ; N2 ,A_ ; N3 X_ Z_ ,A_ ; In addition to the dimensional command, angle command must be specified in

block No. 3. If the angle command is not specified, alarm PS0056, “NO END POINT & ANGLE IN CHF/CNR” is issued. If the coordinates are not specified with an absolute programming, alarm PS0312, “ILLEGAL COMMAND IN DIRECT DRAWING DIMENSIONS PROGRAMMING” is issued.

10 In the tool nose radius compensation mode, a block in which only the angle command is specified in direct drawing dimension programming is assumed to be a block with no move command. For details of compensation when sequential blocks with no move command are specified, see the explanation of tool nose radius compensation.

11 If two or more blocks with no move command are specified between sequential commands of direct drawing dimension programming, alarm PS0312 is issued.

12 When bit 4 (CCR) of parameter No. 3405 is set to 1, address A in the G76 (multiple threading cycle) block specifies the tool nose angle.

When A or C is used as an axis name, it cannot be used in the angle or chamfering command in direct drawing dimension programming. Use ,A_ or ,C_ (when bit 4 (CCR) of parameter No. 3405 is set to 0).

13 In a multiple repetitive canned cycle, in blocks with sequence numbers between those specified at P and Q, a program using direct drawing dimension programming can be used. The block with the last sequence number specified at Q must not be an intermediate block of these specified blocks.

B-64484EN-1/02 PROGRAMMING

— 125 —

4.FUNCTIONS TO SIMPLIFYPROGRAMMING

Example

22°

180

301 × 45°

10°

R20

φ100

φ300

φ60

(Diameter specification, metric input)

N001 G50 X0.0 Z0.0 ;N002 G01 X60.0 ,A90.0 ,C1.0 F80 ;N003 Z-30.0 ,A180.0 ,R6.0 ;N004 X100.0 ,A90.0 ;N005 ,A170.0 ,R20.0 ;N006 X300.0 Z-180.0 ,A112.0 ,R15.0 ;N007 Z-230.0 ,A180.0 ;

R15

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 126 —

5 COMPENSATION FUNCTION Chapter 5, «COMPENSATION FUNCTION», consists of the following sections: 5.1 TOOL OFFSET…………………………………………………………………………………………………………………126 5.2 OVERVIEW OF TOOL NOSE RADIUS COMPENSATION (G40-G42)………………………………..136 5.3 OVERVIEW OF CUTTER COMPENSATION (G40-G42) ……………………………………………………148 5.4 DETAILS OF CUTTER OR TOOL NOSE RADIUS COMPENSATION………………………………..154 5.5 VECTOR RETENTION (G38)……………………………………………………………………………………………205 5.6 CORNER CIRCULAR INTERPOLATION (G39) ………………………………………………………………..206 5.7 EXTENDED TOOL SELECTION ………………………………………………………………………………………208 5.8 AUTOMATIC TOOL OFFSET (G36, G37) …………………………………………………………………………211 5.9 COORDINATE SYSTEM ROTATION (G68.1, G69.1) ………………………………………………………..214 5.10 ACTIVE OFFSET VALUE CHANGE FUNCTION BASED ON MANUAL FEED …………………218

5.1 TOOL OFFSET Tool offset is used to compensate for the difference when the tool actually used differs from the imagined tool used in programming (usually, standard tool).

Offset amounton X axis

Standard tool

Actual tool

Offset amounton Z axis

Fig. 5.1 (a) Tool offset

5.1.1 Tool Geometry Offset and Tool Wear Offset Tool geometry offset and tool wear offset are possible to divide the tool offset to the tool geometry offset for compensating the tool shape or tool mounting position and the tool wear offset for compensating the tool nose wear. The tool geometry offset value and tool wear offset value can be set individually. When these values are not distinguished from each other, the total of the values is set as the tool offset value.

NOTE Tool geometry offset and tool wear offset are optioned.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 127 —

Point on the program

X axisgeometryoffsetvalue

X axiswearoffsetvalue

Z axisgeometryoffsetvalue

Z axiswearoffsetvalue

Offsetamounton X axis

Offsetamounton Z axis

Point on the program

Imaginary tool

Fig. 5.1.1 (a) If tool geometry offset and tool wear offset are distinguished

from each other (left) and if they are not (right)

5.1.2 T Code for Tool Offset

Format Select a tool with a numeric value after a T code. A part of the numeric value is used as a tool offset number for specifying data such as a tool offset value. The following selections can be made according to the specification method and parameter setting:

Meaning of T code (*1) Bit 1 (LGN) of parameter No.

5002=0 Bit 1 (LGN) of parameter No.

5002=1

Parameter setting for specifying of offset No. (*2)

A tool wear offset number is specified using the lower one digit of a T code.

T x x x x x x x y xxxxxxx : Tool selection y : Tool wear and tool

geometry offset

T x x x x x x x y xxxxxxx : Tool selection and tool

geometry offset y : Tool wear offset When parameter No. 5028 is set to 1

A tool wear offset number is specified using the lower two digits of a T code.

T x x x x x x y y xxxxxx : Tool selection yy : Tool wear and tool

geometry offset

T x x x x x x y y xxxxxx : Tool selection and tool

geometry offset yy : Tool wear offset When parameter No. 5028 is set to 2

A tool wear offset number is specified using the lower three digits of a T code.

T x x x x x y y y xxxxx : Tool selection yyy : Tool wear and tool

geometry offset

T x x x x x y y y xxxxx : Tool selection and tool

geometry offset yyy : Tool wear offset When parameter No. 5028 is set to 3

*1 The maximum number of digits of a T code can be specified using parameter No. 3032. (1 to 8

digits) *2 When parameter No. 5028 is set to 0, the number of digits of a T code used for offset number

specification depends on the number of tool offsets. Example) When the number of tool offsets is 1 to 9: Lower one digit When the number of tool offsets is 10 to 99: Lower two digits When the number of tool offsets is 100 to 999: Lower three digits

5.1.3 Tool Selection Tool selection is made by specifying the T code corresponding to the tool number. Refer to the machine tool builder’s manual for the relationship between the tool selection number and the tool.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 128 —

5.1.4 Offset Number Tool offset number has two meanings. It is specifies the offset distance corresponding to the number that is selected to begin the offset function. A tool offset number of 0 indicates that the offset amount is 0 and the offset is cancelled.

5.1.5 Offset

Explanation — Offset methods

Two methods are available to geometry offset and wear compensation, offset with tool movement and compensation with coordinate shift. Which offset method to select can be specified with bit 2 (LWT) and bit 4 (LGT) of parameter No. 5002. If, however, the tool geometry and wear offset options are not provided, offset with tool movement is assumed unconditionally.

Parameter Tool geometry and wear offset

options Compensation element LWT=0

LGT=0 LWT=1 LGT=0

LWT=0 LGT=1

LWT=1 LGT=1

Not provided Wear and geometry not distinguished

Tool movement

Wear compensation Tool movement Coordinate shift Tool movement Coordinate shiftProvided

Geometry compensation Coordinate shift Coordinate shift Tool movement Tool movement

— Offset with tool movement The tool path is offset by the X, Y, and Z tool offset values for the programmed path. The tool offset distance corresponding to the number specified by the T code is added to or subtracted from the end position of each programmed block. The vector with tool offset X, Y, and Z is called the offset vector. Offset is the same as the offset vector.

This move command blockcontains the offset commandwith T code

Tool path after offset

Programmed path

Offset by tool offset X, Z (offset vector)

Offset operation with tool movement

NOTE 1 When G50 X_Z_T_ ; is specified, the tool is not moved. The coordinate system in which the coordinate value of the tool position is (X,Z)

is set. The tool position is obtained by subtracting the offset value corresponding to the tool offset number specified in the T code.

2 The G codes in the 00 group other than G50 must not be specified in the same block as that containing a T code. If one of G28, G29, G30, G30.1, and G53 is specified in the same block as that containing a T code, alarm PS0245, “T-CODE NOT ALLOWED IN THIS BLOCK”, is issued.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 129 —

— Offset with coordinate shift The workpiece coordinate system is shifted by the X, Y, and Z tool offset amounts. Namely, the offset amount corresponding to the number designated with the T code is added to or subtracted from the absolute coordinates.

Programmed path after workpiececoordinate system shift

The movement to this point isby an absolute command.

Tool path after offset

Programmed path beforeworkpiece coordinate system shift

Offset amount by offset inX, Z axis (offset vector)

Offset operation with coordinate shift

— Starting and canceling offset by specifying a T code

Specifying an tool offset number with a T code means to select the tool offset value corresponding to it and to start offset. Specifying 0 as a tool offset number means to cancel offset. For offset with tool movement, whether to start or cancel the offset can be specified with bit 6 (LWN) of parameter No. 5002. For compensation with coordinate shift, the offset is started and canceled when a T code is specified. For the cancellation of geometry compensation, its operation can be selected with bit 5 (LGC) of parameter No. 5002.

Offset method Bit 6 (LWM) of parameter No. 5002=0 Bit 6 (LWM) of parameter No. 5002=1 Tool movement When a T code is specified When an axial movement is specified

Coordinate shift When a T code is specified

(Note that geometry offset can be canceled only if bit 5 (LGC) of parameter No. 5002 = 1.)

— Canceling offset with reset

Tool offset is canceled under one of the following conditions: <1> The power to the CNC is turned off and turned back on <2> The reset button on the MDI unit is pressed <3> A reset signal is input from the machine to the CNC In cases <2> and <3> above, it is possible to select a cancel operation using bit 3 (LVC) of parameter No. 5006 and bit 7 (TGC) of parameter No. 5003.

Parameter Offset method LVC=0

TGC=0 LVC=1 TGC=0

LVC=0 TGC=1

LVC=1 TGC=1

Wear offset Tool movement Geometry offset

Not canceled.Canceled.

(When axial movement is specified)

Not canceled. Canceled.

(When axial movement is specified)

Wear offset Not canceled. Canceled. Not canceled. Canceled. Coordinate shift Geometry offset Not canceled. Not canceled. Canceled. Canceled.

Example

N1 X60.0 Z50.0 T0202 ; Creates the offset vector corresponding to tool offset number 02. N2 Z100.0 ; N3 X200.0 Z150.0 T0200 ; Cancels the offset vector with offset number 0.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 130 —

Tool path after offset

Programmed tool path

Limitation — Helical interpolation (G02, G03)

Tool offset cannot be specified in a block in which helical interpolation is used.

— Thread cutting (G32,G34,G35,G36) 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”, is issued.

— Coordinate system rotation (G68.1) Coordinate system rotation is executed on the command program first, followed by tool offset.

— 3-dimensional coordinate conversion (G68.1) If tool offset is used, tool offset with coordinate shift cannot be used. Offset with tool movement must be specified inside a nest of 3-dimensional coordinate conversion. Example) G68.1 … ; T0101; : T0100; G69.1 … ;

— Workpiece coordinate system preset (G50.3) Performing workpiece coordinate system preset causes tool offset with tool movement to be canceled; this does not cause tool offset with coordinate shift to be canceled.

— Machine coordinate system setting (G53), reference position return (G28), second, third, and fourth reference position return (G30), floating reference position return (G30.1), and manual reference position return

Basically, before performing these commands or operations, cancel tool offset. These operations do not cause tool offset to be canceled. The following actions take place:

When the command or operation is specified

When the next axial movement command is specified

Tool movement The tool offset value is temporarily canceled.

The tool offset value is reflected.

Coordinate shift Coordinates with the tool offset value reflected are assumed.

Coordinates with the tool offset value reflected are assumed.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 131 —

— Offset command in the coordinate system rotation, scaling, or programmable mirror image mode

If tool offset is specified when offset with coordinate system shift is enabled (when bit 2 (LWT) of parameter No. 5002 is set to 1 or bit 4 (LGT) of parameter No. 5002 is set to 0) in the coordinate system rotation, scaling, or programmable mirror image mode, alarm PS0509 is issued. The same alarm is issued when bit 6 (EVO) of parameter No. 5001 is set to 1 and the offset amount is changed.

5.1.6 Y Axis Offset

Overview When the Y axis, one of the basic three axes, is used with a lathe system, this function performs Y axis offset. If the tool geometry and wear offset options are provided, both tool geometry offset and tool wear offset are effective to Y axis offset.

Explanation Y axis offset results in the same operation as tool offset. For an explanation of the operation, related parameters, and the like, refer to the item “Tool Offset.”

5.1.6.1 Support of arbitrary axes for Y axis offset

Overview In a lath system, Y axis offset has been usable with the basic three axes only. This function enables Y axis offset to be used with arbitrary axes other than the Y axis, which is one of the basic three axes.

5.1.7 Second Geometry Tool Offset

Overview To compensate for a difference in tool attachment position or selection position, this function adds second geometry tool offset to the X axis, Y axis, and Z axis with all paths. In contrast to this offset, the ordinary tool geometry offset is called the first geometry tool offset. It is possible to apply a tool offset value (tool wear offset + tool geometry offset) in the reverse direction, using an appropriate signal. This function may be used if the offset value differs even with a single tool for a mechanical reason depending on the mounting position (inside/outside) or the selected position (right/left).

NOTE 1 To use the second geometry tool offset, the geometry and wear offset options

are required. 2 To use the second geometry tool offset for the Y axis, the Y axis offset option is

required.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 132 —

Format • If bit 1 (LGN) of parameter No. 5002 = 1

First geometry tool offset number orfirst + second geometry tool offset numbers

;

Tool wear offset number

(M code that enables second geometry tool offset) ;M

• If bit 1 (LGN) of parameter No. 5002 = 0

T ;

Tool wear offset number + first geometry tool offset number or wear + first + second geometry tool offset numbers

(M code that enables second geometry tool offset) ;M

Explanation — Specification method

Offset using the second geometry tool offset is performed with a program command. Specify the second geometry tool offset with a T code command, and using the second geometry tool offset signal G2SLC, specify whether to set the offset value of the specified tool geometry offset number to the first geometry tool offset only or to the first geometry tool offset plus the second geometry tool offset. If using the first geometry tool offset plus the second geometry tool offset, specify the axis to which the second geometry tool offset is to be applied, using the appropriate one of the second geometry tool offset axis select signal G2X, G2Z, and G2Y. Generally, before a T code command, specify the M code to enable the second geometry tool offset. For details, refer to the manual supplied by the machine tool builder. The same number as the first geometry tool offset number is always selected as the second geometry tool offset number. During execution, the tool offset value for each axis is either of the following: • First geometry tool offset value + tool wear offset value • First geometry tool offset value + second geometry tool offset value + tool wear offset value Example) • The code is a 4-digit code. (The number of digits of a T code is specified with parameter No. 3032.) • The offset type is tool movement (bit 4 (LGT) of parameter No. 5002 = 1). • The lower two digits of the T code is the tool geometry offset number (parameter No. 5028 = 2). • Offset is performed when the T code block is executed (bit 6 (LWM) of parameter No. 5002 = 0). • The X axis data for first geometry tool offset number 1 is 1.000. • The X axis data for second geometry tool offset number 1 is 10.000. • The tool geometry offset number is specified with the tool selection number (bit 1 (LGN) of

parameter No. 5002 = 1). • Signals G2SLC = ‘1’, G2X = ‘1’, and G2Z = G2Y = ‘0’ If T0102 is specified under the above conditions, the upper two digits 01 of the T code cause the first

and second geometry tool offset numbers 1 to be selected, so that the absolute and machine coordinates will be 11.000 on the X axis only.

— Offset data

The data for the second geometry tool offset can be set for each path. The number of items of the data can be set with parameter No. 5024. The data remains stored even after the power is turned off. If the data is to be made common to paths, use the memory common with both 2 path.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 133 —

Example

O (workpiece origin)

T01/Z (first) : 5

T11 to T16/X (second) : 120

T16/Z (second) : — 190

T13/Z (second) : — 70

T12/Z (second) : — 30

T01

T12

T13

T16T11

— — —

—

T11/Z (second) : 10

T01/X (first) : 20First path (standard turret)

Second path(linear turret)

Fig. 5.1.7 (a)

In the machine configuration shown in the Fig. 5.1.7 (a), for the offset data for the tool mounted to the first path (standard turret), set the offset data of the tool itself as the first geometry tool offset data. (The second geometry tool offset data is 0.) For the offset data for the tool mounted to the second path (linear turret), set the offset data of the tool itself as the first geometry tool offset data and the offset data from the workpiece origin at the mounting position as the second geometry tool offset data. Usually, the offset data of the tool itself is measured separately from the offset data at the mounting position, these data can be set separately by using the second geometry tool offset.

First geometry tool offset Second geometry tool offset No. X axis Z axis No. X axis Z axis 01 20.000 5.000 01 0.000 0.000 : : : : : :

10 25.000 8.000 10 0.000 0.000 11 -20.000 5.000 11 120.000 10.000 12 -10.000 3.000 12 120.000 -30.000 13 -15.000 0.000 13 120.000 -70.000 : : : : : :

16 -18.000 7.000 16 120.000 -190.000

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 134 —

5.1.8 4th/5th Axis Offset

Overview This function enables tool offset for the 4th axis and 5th axis following the basic three axes (X, Y, and Z axes). As with tool offsets based on the basic three axes (X, Y, and Z axes), 32 sets of 4th/5th axis tool offsets are available. By specifying the tool geometry offset and tool wear offset options, tool geometry offset and tool wear offset are enabled. Moreover, the number of sets can be increased from 32 to 64, 99, 400, 999, or 2000 by specifying an option. (With the FANUC Series 32i-B, up to 400 sets can be specified.) A tool offset value can be applied to arbitrary axes by setting an axis number (1 to the maximum number of controlled axes) to be used for 4th axis offset in parameter No. 5044 and setting an axis number (1 to the maximum number of controlled axes) to be used for 5th axis offset in parameter No. 5045. By setting bit 1 (NO5) of parameter No. 11400 to 1, 5th axis offset is enabled. If the same axis as used with the Y axis offset function is specified, however, a Y axis offset value is applied to the specified axis, and a 4th axis offset value or 5th axis offset value is invalidated. Tool offset values can be input through an I/O device.

Explanation The operation of 4th/5th axis offset is the same as the operation of tool offset. For the operation, see Section 5.1, «TOOL OFFSET».

Setting of tool offset values with the G10 command By programming, 4th/5th axis offset values can be input.

Format G10 P_ X_ Y_ Z_ R_ Q_ E_ F_ ; or G10 P_ U_ V_ W_ C_ Q_ E_ F_;

P : Offset number 0 : Specifies a workpiece coordinate system shift value. 1 to 999 : Specifies a tool wear offset value. 10000+(1 to 999) : Specifies a tool geometry offset value, with a number (1 to 999)

representing an offset number. X : X axis offset value (absolute) Y : Y axis offset value (absolute) Z : Z axis offset value (absolute) U : X axis offset value (incremental) V : Y axis offset value (incremental) W : Z axis offset value (incremental) R : Tool nose radius compensation value (absolute) C : Tool nose radius compensation value (incremental) Q : Virtual tool nose number E : 4th axis offset value (absolute) F : 5th axis offset value (absolute)

— Explanation

As in the G10 format above, address E for inputting a 4th axis offset value and address F for inputting a 5th axis offset value allow absolute values only to be input.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 135 —

NOTE 1 When compared with the conventional G10 format for changing tool offset

values, address E for specifying a 4th axis offset value and address F for specifying a 5th axis offset value are newly added in the format above.

2 When a program based on the G10 format above is executed, only those offset values that correspond to programmed axis addresses and offset numbers are rewritten.

Limitation

1. This function is a software option. 2. This function supports the inter-path common memory function. 3. This function does not support direct input/counter input of tool offset values. 4. This function does not support offset value writing using a custom macro variable. 5. This function does not support the PMC window function. However, this function supports writing/reading of 4th/5th axis offset values to and from the C

Language Executor. 6. This function does not support external data input. So, no 4th/5th axis offset value can be modified

with a PMC ladder. 7. This function does not support the second geometry tool offset function. 8. This function does not support the tool management function. 9. This function does not support the wrong operation prevention function. 10. This function does not support the program coordinate switch screen function and the offset memory

switch function.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 136 —

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

It is difficult to produce the compensation necessary to form accurate parts when using only the tool offset function due to tool nose roundness in taper cutting or circular cutting. The tool nose radius compensation function compensates automatically for the above errors.

Workpiece

Insufficientdepth ofcutting

Shape processed without toolnose radius compensation

Tool path without compensation

Tool path with compensation

Tool nose

Fig 5.2 (a) Tool path of tool nose radius compensation

5.2.1 Imaginary Tool Nose The tool nose at position A in Fig. 5.2.1 (a) does not actually exist. The imaginary tool nose is required because it is usually more difficult to set the actual tool nose radius center to the start point than the imaginary tool nose. Also when imaginary tool nose is used, the tool nose radius need not be considered in programming. The position relationship when the tool is set to the start point is shown in Fig. 5.2.1 (a).

AStart point

Start point

When programmed using the toolnose center

When programmed using theimaginary tool nose

Fig. 5.2.1 (a) Tool nose radius center and imaginary tool nose

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 137 —

CAUTION In a machine with reference positions, a standard position like the turret center

can be placed over the start point. The distance from this standard position to the nose radius center or the imaginary tool nose is set as the tool offset value.

Setting the distance from the standard position to the tool nose radius center as the offset value is the same as placing the tool nose radius center over the start point, while setting the distance from the standard position to the imaginary tool nose is the same as placing the imaginary tool nose over the standard position. To set the offset value, it is usually easier to measure the distance from the standard position to the imaginary tool nose than from the standard position to the tool nose radius center.

OFX(Tool offsetin X axis)

OFZ(Tool offsetin Z axis)

Setting the distance from the standard positionto the tool nose center as the tool offset value

Setting the distance from the standard position tothe imaginary tool nose center as the tool offsetvalue

The start position is placed over the tool nose center The start position is placed over the imaginary toolnose

OFX(Tool offsetin X axis)

OFZ(Tool offsetin Z axis)

Fig. 5.2.1 (b) Tool offset value when the turret center is placed over the start point

Unless tool nose radius compensation isperformed, the tool nose center path is thesame as the programmed path.

If tool nose radius compensation is used, accuratecutting will be performed.

Tool nose center path

Programmed path

Start-up

Programmed path

Tool nose center path

Fig. 5.2.1 (c) Tool path when programming using the tool nose center

Without tool nose radius compensation, thetool nose radius center path is the same asthe programmed path.

With tool nose radius compensation, accuratecutting will be performed.

Imaginary toolnose path

Start-up

Programmed path Programmed path

Fig. 5.2.1 (d) Tool path when programming using the imaginary tool nose

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 138 —

5.2.2 Direction of Imaginary Tool Nose The direction of the imaginary tool nose viewed from the tool nose center is determined by the direction of the tool during cutting, so it must be set in advance as well as offset values. The direction of the imaginary tool nose can be selected from the eight specifications shown in the Fig. 5.2.2 (a) below together with their corresponding codes. Fig. 5.2.2 (a) illustrates the relation between the tool and the start point. The following apply when the tool geometry offset and tool wear offset option are selected.

Imaginary tool nose number 1 Imaginary tool nose number 2

Imaginary tool nosenumber 3

Imaginary tool nosenumber 4

Imaginary tool nose number 5 Imaginary tool nose number 6

Imaginary tool nose number 7 Imaginary tool nose number 8

ZG18

XG17

YG19

Fig. 5.2.2 (a) Direction of imaginary tool nose

Imaginary tool nose numbers 0 and 9 are used when the tool nose center coincides with the start point. Set imaginary tool nose number to address OFT for each offset number. Bit 7 (WNP) of parameter No. 5002 is used to determine whether the tool geometry offset number or the tool wear offset number specifies the direction of the virtual tool nose for tool nose radius compensation.

Imaginary tool nose number 0 or 9

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 139 —

5.2.3 Offset Number and Offset Value

Explanation — Offset number and offset value

Tool nose radius compensation value(Tool nose radius value)

When the tool geometry compensation and tool wear compensation are not provided, offset values become as Table 5.2.3 (a):

Table 5.2.3 (a) Offset number and offset value (example) Offset number Up to 999 sets

OFX (Offset value on X

axis)

OFZ (Offset value on Z axis)

OFR (Tool nose radius compensa-

tion value)

OFT (Direction of imaginary tool

nose)

OFY (Offset value on Y axis)

001 002 003 004 005

0.040 0.060 0.050

: : :

0.020 0.030 0.015

: : :

0.200 0.250 0.120

: : :

1 2 6 : : :

0.030 0.040 0.025

: : :

When the tool geometry compensation and tool wear compensation are provided, the offset values become as Table 5.2.3 (b) and Table 5.2.3 (c):

Table 5.2.3 (b) Tool geometry offset (example)

Geometry offset number

OFGX (X-axis

geometry offset amount)

OFGZ (Z-axis

geometry offset amount)

OFGR (Tool nose radius geometry offset

value)

OFT (Imaginary tool nose direction)

OFGY (Y-axis

geometry offset amount)

G001 G002 G003 G004 G005

10.040 20.060

0 : : :

50.020 30.030

0 : : :

0 0

0.200 : : :

1 2 6 : : :

70.020 90.030

0 : : :

Table 5.2.3 (c) Tool geometry offset (example)

Wear offset number

OFWX (X-axis wear offset

amount)

OFWZ (Z-axis wear

offset amount)

OFWR (Tool nose radius wear offset value)

OFT (Imaginary tool nose direction)

OFWY (Y-axis wear

offset amount)W001 W002 W003 W004 W005

0.040 0.060

0 : : :

0.020 0.030

0 : : :

0 0

0.200 : : :

1 2 6 : : :

0.010 0.020

0 : : :

— Tool nose radius compensation

In this case, the tool nose radius compensation value is the sum of the geometry and wear offset values. OFR=OFGR+OFWR

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 140 —

— Imaginary tool nose direction

The imaginary tool nose direction is common to geometry and wear offsets.

— Command of offset value A offset number is specified with the same T code as that used for tool offset.

NOTE When the geometry offset number is made common to the tool selection by the

bit 1 (LGN) of parameter No. 5002 setting and a T code for which the geometry offset and wear offset number differ from each other is designated, the imaginary tool nose direction specified by the geometry offset number is valid. Example) T0102 OFR=OFGR01+OFWR02 OFT=OFT01

By setting bit 7 (WNP) of parameter No. 5002 appropriately, the imaginary tool nose direction specified with the wear offset number can be made valid.

— Setting range of offset value

The range of values that can be set as a compensation value is either of the Table 5.2.3 (d) and Table 5.2.3 (e), depending on the bits 3 (OFE), 2 (OFD), 1 (OFC), and 0 (OFA) of parameter No. 5042.

Table 5.2.3 (d) Valid compensation range (metric input) OFE OFD OFC OFA Range

0 0 0 1 ±9999.99 mm 0 0 0 0 ±9999.999 mm 0 0 1 0 ±9999.9999 mm 0 1 0 0 ±9999.99999 mm 1 0 0 0 ±999.999999 mm

Table 5.2.3 (e) Valid compensation range (inch input)

OFE OFD OFC OFA Range 0 0 0 1 ±999.999 inch 0 0 0 0 ±999.9999 inch 0 0 1 0 ±999.99999 inch 0 1 0 0 ±999.999999 inch 1 0 0 0 ±99.9999999 inch

The offset value corresponding to the offset number 0 is always 0. No offset value can be set to offset number 0.

5.2.4 Workpiece Position and Move Command In tool nose radius compensation, the position of the workpiece with respect to the tool must be specified.

G code Workpiece position Tool path G40 (Cancel) Moving along the programmed path G41 Right side Moving on the left side the programmed path G42 Left side Moving on the right side the programmed path

The tool is offset to the opposite side of the workpiece.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 141 —

Workpiece

G41

G42 X axis

Z axis

G40

The imaginary tool nose is on theprogrammed path.

Imaginary tool nosenumber 1 to 8

Imaginary tool nosenumber 0

Fig. 5.2.4 (a) Workpiece position

The workpiece position can be changed by setting the coordinate system as shown below.

Workpiece

X axis

Z axisG41 (the workpiece is onthe left side)

G42 (the workpiece is onthe right side)NOTE

If the tool nose radiuscompensation value is negative,the workpiece position is changed.

Fig. 5.2.4 (b) When the workpiece position is changed

G40, G41, and, G42 are modal. Don’t specify G41 while in the G41 mode. If you do, compensation will not work properly. Don’t specify G42 while in the G42 mode for the same reason. G41 or G42 mode blocks in which G41 or G42 are not specified are expressed by (G41) or (G42) respectively.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 142 —

CAUTION If the sign of the compensation value is changed from plus to minus and vice

versa, the offset vector of tool nose radius compensation is reversed, but the direction of the imaginary tool tip does not change. For a use in which the imaginary tool tip is adjusted to the starting point, therefore, do not change the sign of the compensation value for the assumed program.

Explanation

— Tool movement when the workpiece position does not change When the tool is moving, the tool nose maintains contact with the workpiece.

(G42)(G42) (G42)

Enlargeddiagram

Fig. 5.2.4 (c) Tool movement when the workpiece position does not change

— Tool movement when the workpiece position changes The workpiece position against the tool changes at the corner of the programmed path as shown in the Fig. 5.2.4 (d).

Workpieceposition

G42

G42G41

G41

A B C

Fig. 5.2.4 (d) Tool movement when the workpiece position changes

Although the workpiece does not exist on the right side of the programmed path in the above case, the existence of the workpiece is assumed in the movement from A to B. The workpiece position must not be changed in the block next to the start-up block. In the above example, if the block specifying motion from A to B were the start-up block, the tool path would not be the same as the one shown.

— Start-up The block in which the mode changes to G41 or G42 from G40 is called the start-up block. G40 _ ; G41 _ ; (Start-up block)

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 143 —

Transient tool movements for offset are performed in the start-up block. In the block after the start-up block, the tool nose center is positioned Vertically to the programmed path of that block at the start point.

G40

(G42)G42 (Start-up)

Fig. 5.2.4 (e) Start-up

— Offset cancel

The block in which the mode changes to G40 from G41 or G42 is called the offset cancel block. G41 _ ; G40 _ ; (Offset cancel block) The tool nose center moves to a position vertical to the programmed path in the block before the cancel block. The tool is positioned at the end position in the offset cancel block (G40) as shown below.

G40

(G42)

End position

Fig. 5.2.4 (f) Offset cancel

— Changing the compensation value

In general, the compensation value is to be changed when the tool is changed in offset cancel mode. If the compensation value is changed in offset mode, however, the vector at the end point of the block is calculated using the compensation value specified in that same block. The same applies if the imaginary tool nose direction and the tool offset value are changed.

Calculated from the compensationvalue specified in block N6.

Calculated from the compensationvalue specified in block N7.

N8N6

Programmed path

Fig. 5.2.4 (g) Changing the compensation value

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 144 —

— Specification of G41/G42 in G41/G42 mode When a G41 or G42 code is specified again in G41/G42 mode, the tool nose center is positioned vertical to the programmed path of the preceding block at the end position of the preceding block.

G42(G42)

(G42)

G42 W-500.0 U-500.0 ;

Fig. 5.2.4 (h) Specification of G41/G42 in G41/G42 mode In the block that first changes from G40 to G41/G42, the above positioning of the tool nose center is not performed.

— Tool movement when the moving direction of the tool in a block which includes a G40 (offset cancel) command is different from the direction of the workpiece

When you wish to retract the tool in the direction specified by X(U) and Z(W) canceling the tool nose radius compensation at the end of machining the first block in the Fig. 5.2.4 (i), specify the following : G40 X(U) _ Z(W) _ I _ K _ ; where I and K are the direction of the workpiece in the next block, which is specified in incremental mode.

(G42)

G40 U_ W_ I_ K_ ;

G40

I, K

U, WMoving direction of tool

Fig. 5.2.4 (i) If I and K are specified in the same block as G40

Thus, this prevents the tool from overcutting, as shown in Fig. 5.2.4 (j).

G40 U_ W_ ;

(G42)

G40

U,W Actual move command

Fig. 5.2.4 (j) Case in which overcutting occurs in the same block as G40

The workpiece position specified by addresses I and K is the same as that in the preceding block. Specify I_K_; in the same block as G40. If it is specified in the same block as G02 or G03, it is assumed to be the center of the arc. G40 X_ Z_ I_ K_ ; Tool nose radius compensation G02 X_ Z_ I_ K_ ; Circular interpolation

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 145 —

If I and/or K is specified with G40 in the offset cancel mode, the I and/or K is ignored. The numeral is followed I and K should always be specified as radius values. G40 G01 X_ Z_ ; G40 G01 X_ Z_ I_ K_ ; Offset cancel mode (I and K are ineffective.)

Example

Z120

200

30 150

φ60

φ300

<1><2>

<3>

(G40 mode) <1> G42 G00 X60.0 ; <2> G01 X120.0 W-150.0 F10 ; <3> G40 G00 X300.0 W150.0 I40.0 K-30.0 ;

5.2.5 Notes on Tool Nose Radius Compensation

Explanation — Blocks without a move command that are specified in offset mode

<1> M05 ; M code output <2> S210 ; S code output <3> G04 X10.0 ; Dwell <4> G22 X100000 ; Machining area setting <5> G01 U0 ; Feed distance of zero <6> G98 ; G code only <7> G10 P01 X10.0 Z20.0 R0.5 Q2 ; Offset change If the number of such blocks consecutively specified is more than N-2 blocks (where N is the number of blocks to read in offset mode (parameter No. 19625)), the tool arrives at the position vertical to this block at the end point of the previous block. If the feed distance is 0 (<5>), this applies even if only one block is specified.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 146 —

(G42 mode)N6 W100.0 ;N7 S21 ;N8 M04 ;U9 U-100.0 W100.0 ;(Number of blocks to be readin offset mode = 3)

N6 N7 N8

N9Tool nose center path

Programmed path

Fig. 5.2.5 (a)

Overcutting may, therefore, occur in the Fig. 5.2.5 (a).

— Tool nose radius compensation with G90 or G94 The tool nose center path and the offset direction are as shown below if tool nose radius compensation is applied. At the cycle start point, the offset vector disappears, and offset starts up with tool movement from the cycle start point. In addition, during a return to the cycle start point, the offset vector disappears temporarily, and offset is applied again with the next move command. The offset direction is determined by the cutting pattern, regardless of G41 or G42.

— Outer/inner turning cycle (G90) Tool nose radius center path Offset direction

Total tool nose

Tool nose radiuscenter path

Programmed path

5 7

16 2

Total toolnose

Total tool nose

— End cutting cycle (G94)

Total tool nose

Tool nose radiuscenter path

Programmed path

5 7

1 6 2

Total toolnose

Total tool nose

Tool nose radius center path Offset direction

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 147 —

— Difference from Series 16i/18i/21i NOTE The offset direction is the same as that of Series 16i/18i/21i, but the tool nose

radius center path is different. • For this CNC

The operation is the same as that performed if the canned cycle operation is replaced with G00 or G01, start-up is performed in the first block for movement from the start point, and offset cancel is performed in the last block for returning to the start point.

• For Series 16i/18i/21i The operation with the block for movement from the start point and the last block for returning to the start point differs from that of this CNC. For details, refer to the Series 16i/18i/21i Operator’s Manual.

— Tool nose radius compensation with G71 to G73

Tool nose radius compensation performed with G71 (outer surface rough cutting cycle or traverse grinding cycle), G72 (end rough cutting cycle or traverse direct constant-size grinding cycle), and G73 (closed loop cutting cycle or oscillation direct constant-size grinding cycle), see the explanations of the respective cycles.

— Tool nose radius compensation with G74 to G76 and G92 With G74 (end cutting off cycle), G75 (outer/inner surface cutting off cycle), G76 (multiple threading cycle), and G92 (threading cycle), tool nose radius compensation cannot be applied.

— Tool nose radius compensation when chamfering is performed Movement after compensation is shown Fig. 5.2.5 (b).

(G42)

(G41)

Programmed path

(G42 mode)G01 W-20.0 I10.0;U20.0;

Fig. 5.2.5 (b)

— Tool nose radius compensation when a corner arc is inserted

Movement after compensation is shown Fig. 5.2.5 (c).

(G42)

(G41)

Programmed path

(G42 mode)G01 W-20.0 R10.0;U20.0;

Fig. 5.2.5 (c)

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 148 —

5.3 OVERVIEW OF CUTTER COMPENSATION (G40-G42) When the tool is moved, the tool path can be shifted by the radius of the tool (Fig. 5.3 (a)). To make an offset as large as the radius of the tool, CNC first creates an offset vector with a length equal to the radius of the tool (start-up). The offset vector is perpendicular to the tool path. The tail of the vector is on the workpiece side and the head positions to the center of the tool. If a linear interpolation or circular interpolation command is specified after start-up, the tool path can be shifted by the length of the offset vector during machining. To return the tool to the start point at the end of machining, cancel the cutter compensation mode.

Start-up

Cuttercompensationcancel

Fig. 5.3 (a) Outline of cutter compensation

Format

— Start up (tool compensation start) G00(or G01)G41(or G42) IP_T_;

G41 : Cutter compensation left (Group 07) G42 : Cutter compensation right (Group 07) IP_ : Command for axis movement T_ : Same T code as that of tool offset

— Cutter compensation cancel (offset mode cancel)

G40 IP_; G40 : Cutter compensation cancel (Group 07) (Offset mode cancel) IP_ : Command for axis movement

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 149 —

— Selection of the offset plane Offset plane Command for plane selection IP_

XpYp G17 ; Xp_Yp_ ZpXp G18 ; Xp_Zp_ YpZp G19 ; Yp_Zp_

Explanation

— Offset cancel mode At the beginning when power is applied the control is in the offset cancel mode. In the offset cancel mode, the vector is always 0, and the tool center path coincides with the programmed path.

— Start-up When a cutter compensation command (G41 or G42) is specified in the offset cancel mode, the CNC enters the offset mode. Moving the tool with this command is called start-up. Specify positioning (G00) or linear interpolation (G01) for start-up. If circular interpolation (G02, G03) or involute interpolation (G02.2, G03.2) is specified, alarm PS0034, “NO CIRC ALLOWED IN STUP/EXT BLK” occurs. For the start-up and subsequent blocks, the CNC prereads as many blocks as the number of preread blocks set in the parameter No. 19625.

— Offset mode In the offset mode, compensation is accomplished by positioning (G00), linear interpolation (G01), or circular interpolation (G02, G03). If three or more blocks that move the tool cannot be read in offset mode, the tool may make either an excessive or insufficient cut. If the offset plane is switched in the offset mode, alarm PS0037, “CAN NOT CHANGE PLANE IN G41/G42” occurs and the tool is stopped.

— Offset mode cancel In the offset mode, when a block which satisfies any one of the following conditions is executed, the CNC enters the offset cancel mode, and the action of this block is called the offset cancel. 1. G40 has been commanded. 2. 0 has been commanded as the offset number for cutter compensation (T code). When performing offset cancel, circular arc commands (G02 and G03) and involute commands (G02.2 and G03.2) are not available. If these commands are specified, an alarm PS0034 is generated and the tool stops. In the offset cancel, the control executes the instructions in that block and the block in the cutter compensation buffer. In the meantime, in the case of a single block mode, after reading one block, the control executes it and stops. By pushing the cycle start button once more, one block is executed without reading the next block. Then the control is in the offset cancel mode, and normally, the block to be executed next will be stored in the buffer register and the next block is not read into the buffer for cutter compensation.

Offset cancel mode Offset mode

Start up

Offset mode cancel

(G41/G42)

(G40/T0)

Fig. 5.3 (b) Changing the offset mode

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 150 —

— Change of the cutter compensation value In general, the cutter compensation value shall be changed in the offset cancel mode, when changing tools. If the cutter compensation value is changed in offset mode, the vector at the end point of the block is calculated for the new cutter compensation value.

Calculated from the cutter compensation value in the block N6

Calculated from the cutter compensation value in the block N7

N7N6 N8Programmed path

Fig. 5.3 (c) Changing the cutter compensation value

— Positive/negative cutter compensation value and tool center path

If the compensation value is negative (–), distribution is made for a figure in which G41’s and G42’s are all replaced with each other on the program. Consequently, if the tool center is passing around the outside of the workpiece, it will pass around the inside, and vice versa. Fig. 5.3 (d) shows one example. Generally, the compensation value is programmed to be positive (+). When a tool path is programmed as in <1>, if the compensation value is made negative (–), the tool center moves as in <2>, and vice versa. Consequently, the same program permits cutting both male and female shapes, and any gap between them can be adjusted by the selection of the compensation value. Applicable if start-up and cancel is A type. (See the descriptions about the start-up of cutter compensation.)

<1> <2>

Programmed path

Tool center path

Fig. 5.3 (d) Tool center paths when positive and negative cutter compensation values are specified

— Cutter compensation value setting

Assign a cutter compensation values to the T codes on the MDI unit.

NOTE The cutter compensation value for which the T code corresponds to 0 always

means 0. It is not possible to set the cutter compensation value corresponding to T0.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 151 —

— Valid compensation value range The valid range of values that can be set as a compensation value is either of the following, depending on the bits 3 (OFE), 2 (OFD), 1 (OFC), and 0 (OFA) of parameter No. 5042.

Valid compensation range (metric input) OFE OFD OFC OFA Range

0 0 0 1 ±9999.99 mm 0 0 0 0 ±9999.999 mm 0 0 1 0 ±9999.9999 mm 0 1 0 0 ±9999.99999 mm 1 0 0 0 ±999.999999 mm

Valid compensation range (inch input)

OFE OFD OFC OFA Range 0 0 0 1 ±999.999 inch 0 0 0 0 ±999.9999 inch 0 0 1 0 ±999.99999 inch 0 1 0 0 ±999.999999 inch 1 0 0 0 ±99.9999999 inch

The compensation value corresponding to offset No. 0 always means 0. It is not possible to set the compensation value corresponding to offset No. 0.

— Offset vector The offset vector is the two dimensional vector that is equal to the cutter compensation value assigned by T code. It is calculated inside the control unit, and its direction is up-dated in accordance with the progress of the tool in each block. The offset vector is deleted by reset.

— Specifying a cutter compensation value Specifying a cutter compensation value is accomplished by specifying an offset number, using the same T code as that for specifying tool offset.

— Plane selection and vector Offset calculation is carried out in the plane determined by G17, G18 and G19, (G codes for plane selection). This plane is called the offset plane. Compensation is not executed for the coordinate of a position which is not in the specified plane. The programmed values are used as they are. In simultaneous 3 axes control, the tool path projected on the offset plane is compensated. The offset plane is changed during the offset cancel mode. If it is performed during the offset mode, an alarm PS0037 is displayed and the machine is stopped.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 152 —

Example

Y axis

X axis Unit : mm

Start point

650RC2 (1550,1150)

650R

C3 (-150,1150)

250R

C1(700,1300)

P4(500,1150) P5(900,1150)

P6(950,900)

P9(700,650)P8(1150,550)

P7(1150,900)

P1(250,550)

P3(450,900)P2(250,900)

N3N4

N6N7

N9N10

N11

G50 X0 Y0 Z0 ;……………………………………..Specifies absolute coordinates. The tool is positioned at the start point (X0, Y0, Z0). N1 G17 G00 G41 T0707 X250.0 Y550.0 ; ….Starts cutter compensation (start-up). The tool is shifted to the left of the programmed path by

the distance specified in T07. In other words the tool path is shifted by the radius of the

tool (offset mode) because T07 is set to 15 beforehand (the radius of the tool is 15 mm).

N2 G01 Y900.0 F150 ; ……………………………….Specifies machining from P1 to P2. N3 X450.0 ; ………………………………………………..Specifies machining from P2 to P3. N4 G03 X500.0 Y1150.0 R650.0 ;………………Specifies machining from P3 to P4. N5 G02 X900.0 R-250.0 ; …………………………..Specifies machining from P4 to P5. N6 G03 X950.0 Y900.0 R650.0 ; ………………..Specifies machining from P5 to P6. N7 G01 X1150.0 ; ………………………………………Specifies machining from P6 to P7. N8 Y550.0 ; ………………………………………………..Specifies machining from P7 to P8. N9 X700.0 Y650.0 ; ……………………………………Specifies machining from P8 to P9.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 153 —

N10 X250.0 Y550.0 ; ……………………………………Specifies machining from P9 to P1. N11 G00 G40 X0 Y0 ;…………………………………..Cancels the offset mode. The tool is returned to the start point (X0, Y0, Z0).

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 154 —

5.4 DETAILS OF CUTTER OR TOOL NOSE RADIUS COMPENSATION

5.4.1 Overview The following explanation focuses on tool nose radius compensation, but applies to cutter compensation as well. Examples in which XY planes are used, however, apply to cutter compensation only.

— Tool nose radius center offset vector The tool nose radius center offset vector is a two dimensional vector equal to the offset value specified in a T code, and the vector is calculated in the CNC. Its dimension changes block by block according to tool movement. This offset vector (simply called vector herein after) is internally crated by the control unit as required for proper offsetting and to calculate a tool path with exact offset (by tool nose radius) from the programmed path. This vector is deleted by resetting. The vector always accompanies the tool as the tool advances. Proper understanding of vector is essential to accurate programming. Read the description below on how vectors are created carefully.

— G40, G41, G42 G40, G41 or G42 is used to delete or generate vectors. These codes are used together with G00, G01, G02, or G32 to specify a mode for tool motion (Offsetting).

G code Workpiece position Function G40 Neither Tool nose radius compensation cancel G41 Right Left offset along tool path G42 Left Right offset along tool path

G41 and G42 specify an offset mode, while G40 specifies cancellation of the offset.

— Inner side and outer side When an angle of intersection of the tool paths specified with move commands for two blocks on the workpiece side is over 180°, it is referred to as «inner side.» When the angle is between 0° and 180°, it is referred to as «outer side.»

αWorkpiece α

Programmed path

Inner side

180°≤a 0°≤α<180°

Outer side

Workpiece

Programmed path

— Outer corner connection method If the tool moves around an outer corner in tool nose radius compensation mode, it is possible to specify whether to connect compensation vectors with linear interpolation or with circular interpolation, using bit 2 (CCC) of parameter No. 19607.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 155 —

Vectors are connected with linearinterpolation.

Vectors are connected with circularinterpolation.

Fig. 5.4.1 (a) Linear connection type Fig.5.4.1 (b) Circular connection type

[Bit 2 (CCC) of parameter No. 19607 = 0] [Bit 2 (CCC) of parameter No. 19607 = 1]

— Cancel mode The tool nose radius compensation enters the cancel mode under the following conditions. (The system may not enter the cancel mode depending on the machine tool.) (1) Immediately after the power is turned on (2) After the key on the MDI unit is pushed (3) After a program is forced to end by executing M02 or M30 (4) After the tool nose radius compensation cancel command (G40) is exercised In the cancel mode, the magnitude of a compensation vector is 0 at all times and the path of the virtual tool nose matches the programmed path. A program must end in cancel mode. If it ends in the tool nose radius compensation mode, the tool cannot be positioned at the end point, and the tool stops at a location the compensation vector length away from the end point.

NOTE The operation performed when a reset operation is performed during tool nose

radius compensation varies according to the setting of bit 6 (CLR) of parameter No. 3402. • When CLR=0

The reset state is set. The modal information of G41/G42 in group 07 is preserved. To perform tool nose radius compensation, however, an offset number (T code) needs to be specified again.

• When CLR=1 The cleared state is set. The modal information of G40 in group 07 is preserved. To perform tool nose radius compensation, G41/G42 and an offset number (T code) need to be specified.

— Start-up

When a block which satisfies all the following conditions is executed in cancel mode, the CNC enters the offset mode. Control during this operation is called start-up. (1) G41 or G42 is contained in the block, or has been specified to place the CNC in the offset mode. (2) 0 < compensation number of tool nose radius compensation ≤ maximum compensation number (3) Positioning (G00) or linear interpolation (G01) mode (4) A compensation plane axis command with a travel distance of 0 (except start-up type C) is specified. If start-up is specified in circular interpolation (G02, G03) mode, alarm PS0034, “NO CIRC ALLOWED IN STUP/EXT BLK” will occur. Workpiece coordinate system switching (G54 to G59) cannot be specified in the start-up block.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 156 —

As a start-up operation, one of the three types A, B, and C can be selected by setting bits 0 (SUP) and 1 (SUV) of parameter No. 5003 appropriately. The operation to be performed if the tool moves around an inner side is of single type only.

Table 5.4.1 (a) Start-up/cancel operation SUV SUP Type Operation

0 0 Type A A compensation vector is output, which is vertical to the block subsequent to the start-up block and the block preceding the cancel block.

G41

Tool nose radius center path

Programmed path

0 1 Type B A compensation vector is output, which is vertical to the start-up

block and the cancel block. An intersection vector is also output.

G41

Intersection Tool nose radius center path

Programmed path

1 0

1 Type C When the start-up block and the cancel block are blocks without tool

movement, the tool moves by the cutter or tool nose radius compensation value in the direction vertical to the block subsequent to the start-up block and the block preceding the cancel block.

G41

Intersection Tool nose radius center path

Programmed pathN3Programmedpath

For a block with tool movement, the tool follows the SUP setting: If it is 0, type A is assumed and if 1, type B is assumed.

— Reading input commands in tool nose radius compensation mode

In tool nose radius compensation mode, input commands are read from usually three blocks and up to eight blocks depending on the setting of parameter No. 19625 to perform intersection calculation or an interference check, described later, regardless of whether the blocks are with or without tool movement, until a cancel command is received. To perform intersection calculation, it is necessary to read at least two blocks with tool movement. To perform an interference check, it is necessary to read at least three blocks with tool movement. As the setting of parameter No. 19625, that is, the number of blocks to read, increases, it is possible to predict overcutting (interference) for up to more subsequent commands. Increases in blocks to read and analyze, however, cause reading and analysis to take more time.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 157 —

— Bit 0 (SBK) of parameter No. 5000 When bit 0 (SBK) of parameter No. 5000 is set to 1, a single block stop can be performed in a block created internally for tool nose radius compensation. Use this parameter to check a program including tool nose radius compensation.

Single block stop point S

Stop point in a block created internally

Programmed path

Tool nose radius center pathN1 N2

NOTE When an auxiliary function (M code), spindle speed function (S code), tool

function (T code), or second auxiliary function (B code) is specified in the N1 block in the figure above, FIN is not accepted if the tool stops at the stop point in a block created internally (excluding the single block stop point).

— Meaning of symbols

The following symbols are used in subsequent figures: • S indicates a position at which a single block is executed once. • SS indicates a position at which a single block is executed twice. • SSS indicates a position at which a single block is executed three times. • L indicates that the tool moves along a straight line. • C indicates that the tool moves along an arc. • r indicates the cutter or tool nose radius compensation value. • An intersection is a position at which the programmed paths of two blocks intersect with each other

after they are shifted by r. • indicates the center of the tool nose radius.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 158 —

5.4.2 Tool Movement in Start-up When the offset cancel mode is changed to offset mode, the tool moves as illustrated below (start-up):

Explanation — Tool movement around an inner side of a corner (180°≤ α)

G42r

G42

Tool nose radiuscenter path

Start point

Programmed path

Work-piece

Linear→Circular

Start point

Workpiece

Tool nose radius center path

Linear→Linear

Programmed path

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 159 —

— Cases in which the start-up block is a block with tool movement and the tool moves around the outside at an obtuse angle (90°≤ α<180°)

Tool path in start-up has two types A and B, and they are selected by bit 0 (SUP) of parameter No. 5003. Linear→Linear

Programmed path

Tool nose radiuscenter path

G42

Linear→Circular

TypeA

TypeB

G42

Workpiece

Start point

Linear→Linear(Linear connection type)

Linear→Circular(Linear connection type)

Workpiece

Start point

Work-piece

Programmed path

Tool nose radiuscenter path

Tool nose radius center path

Intersection

Workpiece

Programmed path

Start point

G42

Tool nose radius center path

G42

Programmed path

Work-piece

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 160 —

TypeB

Linear→Linear(Circularconnection type)

Linear→Circular(Circularconnection type)

Programmed pathTool nose radius center path

Start point

G42

Workpiecerr

Programmed path

Tool nose radiuscenter path

G42

Workpiece

Start point

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 161 —

— Cases in which the start-up block is a block with tool movement and the tool moves around the outside at an acute angle (α<90°)

Tool path in start-up has two types A and B, and they are selected by bit 0 (SUP) of parameter No. 5003.

G42

S C

TypeA

TypeB

G42L

G42

L L

G42

Linear→Linear

Linear→Circular

Linear→Linear(Linear connection type)

Linear→Circular(Linear connection type)

Workpiece

Work-piece

Workpiece

Work-piece

Start point

Programmed path

Tool nose radius center path

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 162 —

TypeB

Programmed path

αG42

Start pointL

Tool nose radius center path

αG42

Start pointL

Programmed path

Tool nose radius center pathC

Workpiece

Work-piece

Linear→Linear(Circularconnection type)

Linear→Circular(Circularconnection type)

— Tool movement around the outside linear → linear at an acute angle less than 1 degree (α<1°)

G41

(G41)

Start point

Tool nose radius center path

Programmed path

Less than 1 deg

— A block without tool movement specified at start-up For type A and B If the command is specified at start-up, the offset vector is not created. The tool does not operate in a

start-up block.

Programmed path

Tool nose radiuscenter path

G40 … ;

N6 U100.0 W100.0 ;N7 G41 U0 ;N8 U-100.0 ;N9 U-100.0 W100.0 ;

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 163 —

For type C The tool shifts by the compensation value in the direction vertical to the block with tool movement

subsequent to the start-up block.

Programmed path

Tool nose radius center path

Intersection

Without toolmovement

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 164 —

5.4.3 Tool Movement in Offset Mode In offset mode, compensation is performed even for positioning commands, not to speak of linear and circular interpolations. To perform intersection calculation, it is necessary to read at least two blocks with tool movement. If, therefore, two or more blocks with tool movement cannot be read in offset mode because blocks without tool movement, such as auxiliary function independent commands and dwell, are specified in succession, excessive or insufficient cutting may occur because intersection calculation fails. Assuming the number of blocks to read in offset mode, which is determined by parameter No. 19625, to be N and the number of commands in those N blocks without tool movement that have been read to be M, the condition under which intersection calculation is possible is (N — 2) ≥ M. For example, if the maximum number of blocks to read in offset mode is 5, intersection calculation is possible even if up to three blocks without tool movement are specified.

NOTE The condition necessary for an interference check, described later, differs from

this condition. For details, see the explanation of the interference check. If a G or M code in which buffering is suppressed is specified, no subsequent commands can be read before that block is executed, regardless of the setting of parameter No. 19625. Excessive or insufficient cutting may, therefore, occur because of an intersection calculation failure.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 165 —

— Tool movement around the inside of a corner (180°≤ α)

Linear→Linear

Programmed path

IntersectionTool nose radiuscenter path

Workpiece

Linear→Circular

Intersection

Programmed pathTool nose radiuscenter path

Work-piece

Circular→Linear

Intersection

Programmed path

Tool nose radiuscenter path

Circular→Circular

Programmed path

Intersection

Workpiece

Tool nose radiuscenter path

Work-piece

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 166 —

— Tool movement around the inside (α<1°) with an abnormally long vector, linear → linear

Intersection

Programmed path

Tool nose radius center path

Also in case of arc to straight line, straight line to arc and arc to arc, the reader should infer in the same procedure.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 167 —

— Tool movement around the outside corner at an obtuse angle (90°≤α<180°) Linear→Linear(Linearconnection type)

Tool nose radiuscenter path

Programmed path

Workpiece

SIntersection

Work-pieceL

S L

Workpiece

Tool noseradius centerpath

LLS

Intersection

Linear→Circular(Linearconnection type)

Circular→Linear(Linearconnection type)

Circular→Circular(Linearconnection type)

Intersection

Tool nose radiuscenter path

Programmed path

Intersection

Programmed path

Work-piece

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 168 —

Linear→Linear(Circularconnection type)

Linear→Circular(Circularconnection type)

Circular→Linear(Circularconnection type)

Circular→Circular(Circularconnection type)

Tool nose radiuscenter path

Programmed path

Workpiece

Tool nose radiuscenter path

Programmed path

Work-piece

Workpiece

Tool nose radiuscenter path

Programmed path

Tool nose radiuscenter path

Work-piece

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 169 —

— Tool movement around the outside corner at an acute angle (α<90°)

L L

Linear→Linear(Linearconnection type)

Linear→Circular(Linearconnection type)

Circular→Linear(Linearconnection type)

Circular→Circular(Linearconnection type)

Tool nose radiuscenter path

Programmed path

L L

Workpiece

Work-piece

Tool nose radiuscenter path

Programmed path

Tool nose radius center path

Programmed path

Workpiece

αL

Work-piece

Tool nose radius center path Programmed path

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 170 —

Linear→Linear(Circularconnection type)

Linear→Circular(Circularconnection type)

Circular→Linear(Circularconnection type)

Circular→Circular(Circularconnection type)

Tool nose radiuscenter path

Programmed path

Workpiece

Work-piece

Tool nose radiuscenter path

Programmed path

Tool nose radius center path

Programmed path

Workpiece

Work-piece

Tool nose radius center path Programmed path

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 171 —

— When it is exceptional End position for the arc is not on the arc

If the end of a line leading to an arc is not on the arc as illustrated below (Fig. 5.4.3 (a)), the system assumes that the tool nose radius compensation has been executed with respect to an imaginary circle that has the same center as the arc and passes the specified end position. Based on this assumption, the system creates a vector and carries out compensation. The same description applies to tool movement between two circular paths.

Tool nose radius center path

Programmed path

Center of the arc

Imaginary circle

End the arc

r C

Workpiece

Fig. 5.4.3 (a)

There is no inner intersection

If the cutter or tool nose radius compensation value is sufficiently small, the two circular tool center paths made after compensation intersect at a position (P). Intersection P may not occur if an excessively large value is specified for cutter or tool nose radius compensation. When this is predicted, alarm PS0033, “NO INTERSECTION AT CUTTER COMPENSATION” occurs at the end of the previous block and the tool is stopped. In the example shown Fig. 5.4.3 (b), tool center paths along arcs A and B intersect at P when a sufficiently small value is specified for cutter or tool nose radius compensation. If an excessively large value is specified, this intersection does not occur.

r r

When the cutter or tool nose radiuscompensation value is small

When the cutter or tool nose radiuscompensation value is large

Programmed path

Alarm occurs and the tool stops

Center of the arc ACenter of the arc B

Arc A Arc B

Fig. 5.4.3 (b)

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 172 —

— When the center of the arc is identical with the start point or the end position If the center of the arc is identical with the start point or end point, alarm PS0041, “INTERFERENCE IN CUTTER COMPENSATION” is displayed, and the tool will stop at the start point of the preceding block of the arc.

(G41) N5 G01 W50.0 ; N6 W50.0 ; N7 G02 W100.0 I0 K0 ; N8 G01 U-100.0 ;

Alarm is displayed and the tool stops

Programmed path

Tool nose radius center path

N6 N7N5

— Change in the offset direction in the offset mode

The offset direction is decided by G codes (G41 and G42) for cutter or tool nose radius compensation and the sign of the compensation value as follows.

Sign of compensationG code + —

G41 Left side offset Right side offset G42 Right side offset Left side offset

The offset direction can be changed in the offset mode. If the offset direction is changed in a block, a vector is generated at the intersection of the tool nose radius center path of that block and the tool nose radius center path of a preceding block. However, the change is not available in the start-up block and the block following it.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 173 —

— Tool nose radius center path with an intersection Linear→Linear

Linear→Circular

Circular→Linear

Circular→Circular

Programmed path

Tool nose radius center path

r r

G42

G41

Workpiece

Intersection

G41G42

G41

G42

G41

G42

Workpiece

Programmed path

Intersection

Workpiece

Tool nose radius center path

Workpiece

Programmed path

Tool nose radius center path

Intersection

Workpiece

Tool nose radius center path

Workpiece

Intersection

Workpiece

Programmed path

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 174 —

— Tool nose radius center path without an intersection When changing the offset direction in block A to block B using G41 and G42, if intersection with the offset path is not required, the vector normal to block B is created at the start point of block B.

An arc whose end positionis not on the arc

Tool nose radiuscenter path

G41

r r

(G42)

SCenterCenter

Linear→Circular

Tool nose radiuscenter path

Programmed path

Tool nose radiuscenter path

L S

(G41) G42

Programmed path

Tool nose radiuscenter path

Circular→Circular

(G41)

Linear→Linear

Intersection

G41B

G42 (G42)

G42

G41

Workpiece

(G42)

Programmed path

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 175 —

The length of tool center path larger than the circumference of a circle Normally there is almost no possibility of generating this situation. However, when G41 and G42 are changed, or when a G40 was commanded with address I, J, and K this situation can occur. In this case of the Fig. 5.4.3 (c), the cutter compensation is not performed with more than one circle circumference: an arc is formed from P1 to P2 as shown. Depending on the circumstances, an alarm may be displayed due to the «Interference Check» described later. To execute a circle with more than one circumference, the circle must be specified in segments.

(G42)N5 G01 U-700.0 W500.0 ;N6 G41 G02 I-500.0 ;N7 G42 G01 U700.0 W500.0 ;

P1 P2

Tool nose radiuscenter path Programmed path

Fig. 5.4.3 (c)

— Tool nose radius compensation G code in the offset mode

The offset vector can be set to form a right angle to the moving direction in the previous block, irrespective of machining inner or outer side, by commanding the tool nose radius compensation G code (G41, G42) in the offset mode, independently. If this code is specified in a circular command, correct circular motion will not be obtained. When the direction of offset is expected to be changed by the command of tool nose radius compensation G code (G41, G42), see «Change in the offset direction in the offset mode».

A block specified by G42

Linear→Linear

Tool nose radius center path

Circular→Linear

IntersectionS

G42 mode

Programmed path

CIntersectionS

LG42 mode

A block specified by G42

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 176 —

— Command canceling the offset vector temporarily

During offset mode, if G50 (workpiece coordinate system setting) or G52 (local coordinate system setting) is commanded, the offset vector is temporarily cancelled and thereafter offset mode is automatically restored. In this case, without movement of offset cancel, the tool moves directly from the intersecting point to the commanded point where offset vector is canceled. Also when restored to offset mode, the tool moves directly to the intersecting point.

Tool nose radiuscenter path

Programmed path N7G50 block(G41)

N5 G01 U300.0 W700.0 ;N6 U-300.0 W600.0 ;N7 G50 X100.0 Z200.0 ;N8 G01 X400.0 Z800.0 ;

LL L

SN5 N6 N8

Before specifying G28 (reference position return), G29 (return from reference position), G30 (second, third, and fourth reference position returns), G30.1 (floating reference position return), and G53 (machine coordinate system selection) commands, cancel offset mode, using G40. If an attempt is made to specify any of the commands in offset mode, the offset vector temporarily disappears.

— Canned cycles (G90, G92, G94) and multiple repetitive canned cycles (G71 to G76)

See the cautions for the tool nose radius compensation related canned cycles.

Tool nose radiuscenter path

(G42)N5 G01 U50.0 W-60.0 ;N6 W-80.0 ;N7 G90 U-60.0 W-80.0 R-30.0 ;N8 G01 U120.0 W50.0 ;N9 W50.0 ;

N6(G42)N7

Programmed path

— If I, J, and K are specified in a G00/G01 mode block

At the start of tool nose radius compensation or in that mode, by specifying I, J, and K in a positioning mode (G00) or linear interpolation mode (G01) block, it is possible to set the compensation vector at the end point of that block in the direction vertical to that specified by I, J, and K. This makes it possible to change the compensation direction intentionally.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 177 —

IJ type vector (XY plane) The following explains the compensation vector (IJ type vector) to be created on the XY compensation plane (G17 mode). (The same explanation applies to the KI type vector on the G18 plane and the JK type vector on the G19 plane.) As shown in the Fig. 5.4.3 (d) and Fig. 5.4.3 (e), it is assumed that the compensation vector (IJ type vector) is the vector with a size equal to the compensation value and vertical to the direction specified by I and J, without performing intersection calculation on the programmed path. I and J can be specified both at the start of tool nose radius compensation and in that mode. If they are specified at the start of compensation, any start-up type set in the appropriate parameter will be invalid, and an IJ type vector is assumed.

Offset vector direction In G41 mode, the direction specified by I, J, and K is assumed an imaginary tool movement direction, and an offset vector is created vertical to that direction and on the left side.

Compensation vector

I, J, K

Fig. 5.4.3 (d)

In G42 mode, the direction specified by I, J, and K is assumed an imaginary tool movement direction, and an offset vector is created vertical to that direction and on the right side.

Compensation vector

I, J, K

Fig. 5.4.3 (e)

Example

Programmed path

(G40) N10 G41 U100.0 W100.0 K1 T0101 ; N20 G04 X1000 ; N30 G01 F1000 ; N40 S300 ; N50 M50 ; N60 W150.0 ; Note) In N10, a vector is specified with

a size of T1 in the direction vertical to the Z axis, using K1.

If I and J are specified at the start of compensation (with tool movement)

Tool nose radius center path

T1N10

N50N40N30N20 N60

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 178 —

If I and J are specified at the start of compensation (without tool movement)

(G40) N10 G41 K1 T0101 ; N20 U100.0 W100.0 ; N30 W150.0 ; Note) In N10, a vector is specified

with a size of T1 in the direction vertical to the Z axis, using K1.

Tool nose radius center path

Programmed path

N10

N20

N30

(G17 G41 T0101) N10 G00 U150.0 J50.0 ; N20 G02 I50.0 ; N30 G00 U-150.0 ; Note) In N10, a vector is specified

with a size of T1 in the direction vertical to the Y axis, using J50.0.

<1> IJ type vector <2> Vector determined with

intersection calculation

If I and J are specified at the start of compensation (with tool movement)

Path determined with intersection calculation

Programmed path

Tool center path

<1>

<2>

(I,J)

N10 N20 N30

Start-up/cancel type C N10 G41 T0101 G01 F1000 ; N20 U100.0 W100.0 ; N30 K10.0 ; N40 W150.0 ; N50 G40 ;

If I and J are specified in a block without tool movement in compensation mode

N10

N30

N20

N40

N50

S S

Tool nose radius center path

Programmed path

(I, J)

Limitation If an IJ type vector is specified, tool interference may occur due to that vector alone, depending on the direction. If this occurs, no interference alarm will occur, or no interference avoidance will be performed. Overcutting may, therefore, result.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 179 —

Start-up/cancel Type C N10 G42 T0101 F1000 ; N20 W100.0; N30 U100.0 W100.0 K10.0 ; N40 U-100.0 W100.0 ; N50 G40 ;

Tool nose radius center path

Overcutting

Programmed path

N10

N30

N20

N40

N50

(I, J)

— A block without tool movement The following blocks have no tool movement. In these blocks, the tool will not move even if cutter compensation is effected. M05 ; : M code output S21 ; : S code output G04 X10.0 ; : Dwell G22 X100000 ; : Machining area setting G10 P01 X10 Z20 R10.0 ; : Tool nose radius compensation value setting/changing (G18) Y200.0 ; : Move command not included in the offset plane. G98 ;, O10 ;, N20 ; : G, O, and N codes only U0 ; : Move distance is zero.

— A block without tool movement specified in offset mode

Unless the number of blocks without movement consecutively specified is more than N-2 blocks (where N is the number of blocks to read in offset mode (parameter No. 19625)) in offset mode, the vector and the tool nose radius center path will be as usual. This block is executed at the single block stop point.

Programmed path

Block N7 is executed here.

Tool nose radiuscenter path

N6 U100.0 W100.0 ;N7 G04 X10.0 ;N8 W100.0 ;

N7 N8

In offset mode, the number of blocks without movement consecutively specified must not exceed N-2 (where N is the number of blocks to read in offset mode (parameter No. 19625). If commanded, a vector whose length is equal to the offset value is produced in a normal direction to tool motion in earlier block, so overcutting may result.

N6 U100.0 W100.0 ;N7 S21 ;N8 G04 X10.0 ;N9 W100.0 ;(No. of blocks to read inoffset mode = 3)

N7,N8 N9

SSS

Programmed path

Blocks N7 and N8 are executed here.

Tool nose radiuscenter path

— If an M/G code that suppresses buffering is specified If an M/G code that suppresses buffering is specified in offset mode, it is no longer possible to read and analyze subsequent blocks regardless of the number of blocks to read in offset mode, which is determined by parameter No. 19625.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 180 —

Then, intersection calculation and a interference check, described later, are no longer possible. If this occurs, overcutting may occur because a vertical vector is output in the immediately preceding block.

If an M code (M50) that suppresses buffering is not specified

Programmed path

Tool nose radiuscenter path

(G42)N5 G01 U40.0 W40.0 ;N6 W40.0 ; : :

IntersectionL

If an M code (M50) that suppresses buffering is specified

(G42)N5 G01 U40.0 W40.0 ;N6 M50 ;N7 W40.0 ; : :

N6 N7

SSBlock N6 is executed here.

Programmed path

Tool nose radiuscenter path

— Workpiece coordinate system or local coordinate system command in the offset mode

If the local coordinate system (G52) or workpiece coordinate system (G50) is specified in the tool nose radius compensation (G41 or G42) or 3-dimensional cutter compensation (G41.2 to G41.6 or G42.2 to G42.6) mode, G52 or G50 is assumed to be a buffering masked G code. The subsequent blocks are not executed until the G52 or G50 block is executed.

— Corner movement When two or more offset vectors are produced at the end of a block, the tool moves linearly from one vector to another. This movement is called the corner movement. If these vectors almost coincide with each other (the distance of corner movement between the vectors is judged short due to the setting of parameter No. 5010), corner movement is not performed. In this case, the vector to the single block stop point takes precedence and remains, while other vectors are ignored. This makes it possible to ignore the very small movements arising from performing tool nose radius compensation, thereby preventing velocity changes due to interruption of buffering.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 181 —

The vector to the single block stop point remains even if ΔVZ ≤ ΔVlimit and ΔVX ≤ Vlimit. Tool nose radius

center path

ΔVlimit is determined with the setting of parameter (No. 5010). Programmed path

This vector is ignored, if ΔVZ ≤ ΔVlimit and ΔVX ≤ ΔVlimit

S ΔVX

ΔVZ

N1 N1

If the vectors are not judged to almost coincide (therefore, are not erased), movement to turn around the corner is performed. The corner movement that precedes the single block stop point belongs to the previous block, while the corner movement that succeeds the single block stop point belongs to the latter block.

This move belongs to block N7, thus, thefeedrate is equal to that in block N7.

This move belongs to block N6, thus, the feedrate is equalto that in block N6.

N6 N7

However, if the path of the next block is semicircular or more, the above function is not performed. The reason for this is as follows:

(G17)N4 G41 G01 U150.0 V200.0 ;N5 U150.0 V200.0 ;N6 G02 J-600.0 ;N7 G01 U150.0 V-200.0 ;N8 G40 U150.0 V-200.0 ;

Tool center path

P2 P3 P4 P5

Programmed path

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 182 —

If the vector is not ignored, the tool path is as follows: P1 → P2 → P3 → (Circle) → P4 → P5 → P6 But if the distance between P2 and P3 is negligible, the point P3 is ignored. Therefore, the tool path is as follows: P2 → P4 Namely, circle cutting by the block N6 is ignored.

— Interruption of manual operation For manual operation during the offset mode, see «Manual Absolute ON and OFF.»

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 183 —

5.4.4 Tool Movement in Offset Mode Cancel

Explanation — If the cancel block is a block with tool movement, and the tool moves around

the inside (180° ≤ α) Linear→Linear

Circular→Linear

Programmed path Tool nose radius center path

Programmed path

Tool nose radiuscenter path

L S

G40r

Workpiece

G40r

Work-piece

Fig. 5.4.4 (a)

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 184 —

— If the cancel block is a block with tool movement, and the tool moves around the outside at an obtuse angle (90° ≤ α < 180°)

Linear→Linear

TypeA

TypeB

Linear→Linear(Linearconnection type)

Circular→Linear

Circular→Linear(Linearconnection type)

Programmed path

Tool nose radiuscenter path

L S

G40

Workpiece

Programmed path Tool nose radius center path

G40

Work-piece r

Programmed path

Tool nose radiuscenter path

G40

Workpiece

Programmed path Tool nose radius center path

Intersection

G40

Work-piece

Inter-section L

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 185 —

TypeB

Linear→Linear(Circularconnection type)

Circular→Linear(Circularconnection type)

Programmed path

Tool nose radius center pathC S

G40

Workpiece

Programmed path Tool nose radius center path

G40

Work-piece

C S

Fig. 5.4.4 (b)

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 186 —

— If the cancel block is a block with tool movement, and the tool moves around the outside at an acute angle (α<90°)

Linear→Linear

Circular→LinearType

TypeB

Linear→Linear(Linearconnection type)

Circular→Linear(Linearconnection type)

Programmed path

αG40

L S

Tool nose radiuscenter path

αL

Programmed path

Tool nose radiuscenter path

Workpiece

Work-piece

G42

G40

G42

Programmed path

αG40

Tool nose radiuscenter path

Programmed path

Tool nose radiuscenter path

Workpiece

Work-piece

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 187 —

TypeB

Linear→Linear(Circularconnection type)

Circular→Linear(Circularconnection type)

Programmed path

αG40

Tool nose radiuscenter path

Programmed path

Tool nose radiuscenter path

Workpiece

Work-piece

Fig. 5.4.4 (c)

— If the cancel block is a block with tool movement, and the tool moves around

the outside at an acute angle of 1 degree or less in a linear → linear manner (α≤1°)

Programmed path

Tool nose radius center path

G40

(G42)

1° or less

Fig. 5.4.4 (d)

— A block without tool movement specified together with offset cancel

For types A and B In the block preceding the cancel block, a vector is created with a size equal to the cutter or tool nose

radius compensation value in the vertical direction. The tool does not operate in the cancel block. The remaining vectors are canceled with the next move command.

N6 U100.0 W100.0 ;N7 G40 ;N8 U0 W130.0 ;

Tool nose radiuscenter path

N7 N8

LSSProgrammed path

Fig. 5.4.4 (e)

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 188 —

For type C The tool shifts by the compensation value in the direction vertical to the block preceding the cancel

block.

Tool nose radiuscenter path

Programmed path

SG40 (withoutmovement)

Fig. 5.4.4 (f)

— Block containing G40 and I_J_K_ The previous block contains G41 or G42

If a G41 or G42 block precedes a block in which G40 and I_, J_, K_ are specified, the system assumes that the path is programmed as a path from the end position determined by the former block to a vector determined by (I,J), (I,K), or (J,K). The direction of compensation in the former block is inherited.

Programmed path

N1 (G42 mode) ;N2 G40 Xb Za I_ K_ ;

In the N1 block, the tool nose radius center movestowards P.In the N2 block, the tool nose radius center movestowards E.

E(a, b)

Tool nose radius center path

(I, K)

(G42)

Workpiece

G40

Fig. 5.4.4 (g)

In this case, note that the CNC obtains an intersection of the tool path irrespective of whether inner or outer side machining is specified.

Programmed path

Tool nose radiuscenter path

(I, K)

(G42)

G40

Fig. 5.4.4 (h)

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 189 —

When an intersection is not obtainable, the tool comes to the normal position to the previous block at the end of the previous block.

Programmed path

Tool nose radiuscenter path

(I, K)

G40P

(G42)

Fig. 5.4.4 (i)

— Length of the tool center path larger than the circumference of a circle

In the example shown below, the tool does not trace the circle more than once. It moves along the arc from P1 to P2. The interference check function described below may raise an alarm. To make the tool trace a circle more than once, program two or more arcs.

(G17 G41) N5 G01 U100.0 ; N6 G02 J-60.0 ; N7 G40 G01 U50.0 V50.0 I-10.0 J-10.0 ;

Programmed path

Tool nose radius center path

(I, J)N5

Fig. 5.4.4 (j)

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

Explanation — Machining a groove smaller than the diameter of the tool nose

Since the tool nose radius compensation forces the path of the center of the tool nose radius to move in the reverse of the programmed direction, overcutting will result. In this case an alarm is displayed and the CNC stops at the start of the block.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 190 —

Programmed path

Tool nose radiuscenter path

Overcutting if the operation would not stop

Workpiece

An alarm is displayed andthe operation stops

Fig. 5.4.5 (a) Machining a groove smaller than the diameter of the tool nose

— Machining a step smaller than the tool nose radius

For a figure in which a workpiece step is specified with an arc, the tool nose radius center path will be as shown in Fig. 5.4.5 (b). If the step is smaller than the tool nose radius, the tool nose radius center path usually compensated as shown in Fig. 5.4.5 (c) may be in the direction opposite to the programmed path. In this case, the first vector is ignored, and the tool moves linearly to the second vector position. The single block operation is stopped at this point. If the machining is not in the single block mode, the cycle operation is continued. If the step is of linear, no alarm will be generated and cut correctly. However uncut part will remain.

Programmed path

Single block stop point

Tool nose radiuscenter path

Workpiece Arc center

Fig. 5.4.5 (b) Machining a step larger than the tool nose radius

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 191 —

Programmed path

An overcutting will result if the first vector is not ignored.However, tool moves linearly.

Tool nose radius center path

WorkpieceArc center

Single block stop point

Arc

Linear movement

The first vector is ignored

Path to be taken if thevector is not ignored

Fig. 5.4.5 (c) Machining a step smaller than the tool nose radius

— Starting compensation and cutting along the Z-axis

It is usually used such a method that the tool is moved along the Z axis after the cutter compensation (normally XY plane) is effected at some distance from the workpiece at the start of the machining. In the case above, if it is desired to divide the motion along the Z axis into rapid traverse and cutting feed, follow the procedure below. Let us consider the following program, assuming the number of blocks to read in cutter compensation mode (parameter No. 19625) to be 3.

N1 G00 G41 U500.0 V500.0 T0101 ;N3 G01 W-300.0 F100 ;N6 V1000.0 F200 ;

N3:Move command in Z axis (one block)

After compensation

Fig. 5.4.5 (d)

In the program example above (Fig. 5.4.5 (d)), when executing block N1, blocks N3 and N6 are also entered into the buffer storage, and by the relationship among them the correct compensation is performed as in the Fig. 5.4.5 (d). Then, suppose that the block N3 (move command in Z axis) is divided into N3 and N5.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 192 —

N1 G00 G41 U500.0 V500.0 T0101 ; N3 G01 W-250.0 ; N5 G01 W-50.0 F100 ; N6 V1000.0 F200 ;

N3, N5:Move command for the Z axis (two blocks)

After compensation

Workpiece

Fig. 5.4.5 (e)

At this time, because the number of blocks to read is 3, blocks up to N5 can be read at the start of N1 compensation, but block N6 cannot be read. As a result, compensation is performed only on the basis of the information in block N1, and a vertical vector is created at the end of the compensation start block. Usually, therefore, overcutting will result as shown in the Fig. 5.4.5 (e). In such a case, it is possible to prevent overcutting by specifying a command with the exactly the same direction as the advance direction immediately before movement along the Z axis beforehand, after the tool is moved along the Z axis using the above rule.

N1 G00 G41 U500.0 V400.0 T0101 ; N2 V100.0 ; N3 W-250.0 ; N5 G01 W-50.0 F100 ; N6 V1000.0 F200 ;

Workpiece

N6After compensation

N3, N5 : Move command for the Z axis (2 blocks)

Fig. 5.4.5 (f)

As the block N2 has the move command in the same direction as that of the block N6, the correct compensation is performed. Alternatively, it is possible to prevent overcutting in the same way by specifying an IJ type vector with the same direction as the advance direction in the start-up block, as in N1 G00 G41 U500.0 V500.0 I0 J1 T0101;, after the tool has moved along the Z axis.

5.4.6 Interference Check Tool overcutting is called interference. The interference check function checks for tool overcutting in advance. However, all interference cannot be checked by this function. The interference check is performed even if overcutting does not occur.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 193 —

Explanation — Condition under which an interference check is possible

To perform an interference check, it is necessary to read at least three blocks with tool movement. If, therefore, three or more blocks with tool movement cannot be read in offset mode because blocks without tool movement, such as independent auxiliary function and dwell, are specified in succession, excessive or insufficient cutting may occur because an interference check fails. Assuming the number of blocks to read in offset mode, which is determined by parameter No. 19625, to be N and the number of commands in those N blocks without tool movement that have been read to be M, the condition under which an interference check is possible is (N — 3) ≥ M. For example, if the maximum number of blocks to read in offset mode is 8, an interference check is possible even if up to five blocks without tool movement are specified. In this case, three adjacent blocks can be checked for interference, but any subsequent interference that may occur cannot be detected.

— Interference check method Two interference check methods are available, direction check and circular angle check. Bit 1 (CNC) of parameter No. 5008 and bit 3 (CNV) of parameter No. 5008 are used to specify whether to enable these methods.

Table 5.4.6 (a) CNV CNC Operation

0 0 An interference check is enabled, and a direction check and a circular angle check can be performed.

0 1 An interference check is enabled, and only a circular angle check is performed. 1 – An interference check is disabled.

NOTE There are no settings for performing a direction check only.

— Interference reference <1> (direction check)

Assuming the number of blocks to read during tool nose radius compensation to be N, a check is first performed on the compensation vector group calculated in (block 1 — block 2) to be output this time and the compensation vector group calculated in (block N-1 — block N); if they intersect, they are judged to interfere. If no interference is found, a check is performed sequentially in the direction toward the compensation vector group to be output this time, as follows: (Block 1 — block 2) and (block N-2 — block N-1) (Block 1 — block 2) and (block N-3 — block N-2) : : (Block 1 — block 2) and (block 2 — block 3) Even if multiple number of compensation vector groups are generated, a check is performed on all pairs. The judgment method is as follows: For a check on the compensation vector group in (block 1 — block 2) and those in (block N-1 — block N), the direction vector from the specified (end point of block 1) to the (end point of block N-1) is compared with the direction vector from the (point resulting from adding the compensation vector to be checked to the end of block 1) to the (point resulting from adding the compensation vector to be checked to the end of block N-1), and if the direction is 90o or greater or 270o or less, they are judged to intersect and interfere. This is called a direction check.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 194 —

Example of interference standard <1> (If the block 1 end-point vector intersects with the block 7 end-point vector)

Programmed path

The direction differs by180°.

Block 5

Block 6

Tool center path

Block 3

Block 1 Block 8

Block 2

Block 4

Block 7

Fig. 5.4.6 (a)

Example of interference standard <1> (If the block 1 end-point vector intersects with the block 2 end-point vector)

Programmed pathTool nose radiuscenter path

The directions ofthese two paths aredifferent (180°).

Block 1

Block 2

Fig. 5.4.6 (b)

— Interference reference <2> (circular angle check)

In a check on three adjacent blocks, that is, a check on the compensation vector group calculated on (block 1 — block 2) and the compensation vector group calculated on (block 2 — block 3), if block 2 is circular, a check is performed on the circular angle between the start and end points of the programmed path and the circular angle of the start and end point of the post-compensation path, in addition to direction check <1>. If the difference is 180o or greater, the blocks are judged to interfere. This is called a circular angle check.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 195 —

Example of <2> (if block 2 is circular and the start point of the post-compensation arc coincide with the end point)

Programmed pathTool nose radiuscenter path

Block 1

Block 2

Block 3

Programmed path

Fig. 5.4.6 (c)

— When interference is assumed although actual interference does not occur

<1> Depression which is smaller than the cutter or tool nose radius compensation value

Programmedpath Tool nose radius center path

Stopped

Fig. 5.4.6 (d)

There is no actual interference, but since the direction programmed in block B is opposite to that of the path after the tool nose radius compensation, the tool stops and an alarm is displayed.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 196 —

<2> Groove which is smaller than the cutter or tool nose radius compensation value

B C

Stopped

Programmedpath Tool nose radius center path

Fig. 5.4.6 (e)

Like <1>, an alarm is displayed because of the interference as the direction is reverse in block B.

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

Explanation The operation to be performed if an interference check judges that an interference (due to overcutting) occurs can be either of the following two, depending on the setting of bit 5 (CAV) of parameter No. 19607.

Table 5.4.6.1 (a) CAV Function Operation

0 Interference check alarm function An alarm stop occurs before the execution of the block in which overcutting (interference) occurs.

1 Interference check avoidance function

The tool path is changed so that overcutting (interference) does not occur, and processing continues.

5.4.6.2 Interference check alarm function

Explanation — Interference other than those between adjacent three blocks

If the end-point vector of block 1 and the end-point vector of block 7 are judged to interfere as shown in the Fig. 5.4.6.2 (a), an alarm will occur before the execution of block 1 so that the tool stops. In this case, the vectors will not be erased.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 197 —

Block 8

Block 3

Block 4 Block 5

Block 6

Block 2

Stopped

Tool nose radiuscenter path

Programmed path

Block 1

Block 7

Fig. 5.4.6.2 (a)

— Interference between adjacent three blocks

If an interference is judged to occur between adjacent three blocks, the interfering vector, as well as any vectors existing inside of it, is erased, and a path is created to connect the remaining vectors. In the example shown in the Fig. 5.4.6.2 (b), V2 and V5 interfere, so that V2 and V5 are erased, so are V3 and V4, which are inside of them, and V1 is connected to V6. The operation during this time is linear interpolation.

Tool center path

Programmed path

Fig. 5.4.6.2 (b)

If, after vector erasure, the last single vector still interferes, or if there is only one vector at the beginning and it interferes, an alarm will occur immediately after the start of the previous block (end point for a single block) and the tool stops. In the example shown in the Fig. 5.4.6.2 (c), V2 and V3 interfere, but, even after erasure, an alarm will occur because the final vectors V1 and V4 interfere.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 198 —

StoppedTool center path

V4 V1

V3 V2

Programmed path

Fig. 5.4.6.2 (c)

5.4.6.3 Interference check avoidance function

Overview If a command is specified which satisfies the condition under which the interference check alarm function generates an interference alarm, this function suppresses the generation of the interference alarm, but causes a new compensation vector to be calculated as a path for avoiding interference, thereby continuing machining. For the path for avoiding interference, insufficient cutting occurs in comparison with the programmed path. In addition, depending on the specified figure, no path for avoiding interference can be determined or the path for avoiding interference may be judged dangerous. In such a case, an alarm stop will occur. For this reason, it is not always possible to avoid interference for all commands.

Explanation — Interference avoidance method

Let us consider a case in which an interference occurs between the compensation vector between (block 1 — block 2) and the compensation vector between (block N-1 — block N). The direction vector from the end point of block 1 to the end point of block N-1 is called a gap vector. At this time, a post-compensation intersection vector between (block 1 — gap vector) and a post-compensation intersection vector between (gap vector — block N) is determined, and a path connecting them is created.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 199 —

Movement o f block 7

Post-compensation intersection vector between block 1 and gap vector

Post-compensation intersection vector between gap vector and block 8

Post-compensation path

Programmed path

Block 1 Block 8

Block 2

Gap vector

Block 3 Block 6

Block 4 Block 5

In this case, the post-compensation end points of blocks 2 to 6 coincide with the end point of block 1. Thus, after compensation, blocks 2 to 6 will be blocks without tool movement.

Block 7

Fig. 5.4.6.3 (a)

If the post-compensation intersection vector of (block 1 — gap vector) and the post-compensation intersection vector of (gap vector — block N) further intersect, vector erasure is first performed in the same way as in «Interference between adjacent three blocks». If the last vectors that remains still intersects, the post-compensation intersection vector of (block 1 — block N) is re-calculated.

In this case, the post-compensation end points of blocks 2 to 7 coincide with the end point of block 1. Thus, after compensation, blocks 2 to 7 will be blocks without tool movement.

Block 3

Post-compensation intersection vector between block 1 and gap vector

Re-calculation

Block 8

Block 2

Block 3

Block 4 Block 5

Block 6

Block 7

Post-compensation path

Programmed path

Block 8

Block 7

Block 6

Post-compensation intersection between gap vector and block 8

Block 1 Block 1

Post-compensation intersection vector between block 1 and block 8

Gap vector Block 2

Block 4 Block 5

Fig. 5.4.6.3 (b)

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 200 —

If the cutter or tool nose radius compensation value is greater than the radius of the specified arc as shown in the Fig. 5.4.6.3 (c), and a command is specified which results in compensation with respect to the inside of the arc, interference is avoided by performing intersection calculation with an arc command being assumed a linear one. In this case, avoided vectors are connected with linear interpolation.

Programmed path

Post-compensation path

Fig. 5.4.6.3 (c)

— If no interference avoidance vector exists

If the parallel pocket shown in the Fig. 5.4.6.3 (d) is to be machined, the end-point vector of block 1 and the end-point vector of block 2 are judged to interfere, and an attempt is made to calculate, as an interference avoidance vector, the intersection vector of the post-compensation path of block 1 and the post-compensation path of block 3. In this case, because blocks 1 and 3 are parallel to each other, no intersection exists. In this case, an alarm will occur immediately before block 1 and the tool will stop.

Block 1

Block 2

Block 3

Programmed path

Tool center pathStopped

Fig. 5.4.6.3 (d)

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 201 —

If the circular pocket shown in the Fig. 5.4.6.3 (e) is to be machined, the end-point vector of block 1 and the end-point vector of block 2 are judged to interfere, and an attempt is made to calculate, as an interference avoidance vector, the intersection vector of the post-compensation path of block 1 and the post-compensation path of block 3. In this case, because blocks 1 and 3 are circular, no post-compensation intersection exists. In this case, an alarm will occur immediately before block 1 and the tool will stop, as in the previous example.

Programmed path Tool center path

Block 1

Block 2

Block 3

Stopped

Fig. 5.4.6.3 (e)

— If it is judged dangerous to avoid interference

If the acute-angle pocket shown in the Fig. 5.4.6.3 (f) is to be machined, the end-point vector of block 1 and the end-point vector of block 2 are judged to interfere, and an attempt is made to calculate, as an interference avoidance vector, the intersection vector of the post-compensation path of block 1 and the post-compensation path of block 3. In this case, the movement direction of the post-avoidance path extremely differs from the previously specified direction. If the post-avoidance path extremely differs from that of the original command (90° or greater or 270° or less), interference avoidance operation is judged dangerous; an alarm will occur immediately before block 1 and the tool will stop.

Tool center path

Programmed path

Block 1

Block 2

Block 3

Stopped

Post-compensation intersection ofblocks 1 and 3

Fig. 5.4.6.3 (f)

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 202 —

If a pocket in which the bottom is wider than the top, such as that shown in the Fig. 5.4.6.3 (g), is to be machined, the end-point vector of block 1 and the end-point vector of block 2 are judged to interfere, and an attempt is made to calculate, as an interference avoidance vector, the intersection vector of the post-compensation path of block 1 and the post-compensation path of block 3. In this case, the relation between blocks 1 and 3 is judged an outer one, the post-avoidance path results in overcutting as compared with the original command. In such a case, interference avoidance operation is judge dangerous; an alarm will occur immediately before block 1 and the tool will stop.

Tool center path

Programmed path

Post-compensation intersectionof blocks 1 and 3

Block 1

Block 2

Block 3

Stopped

Fig. 5.4.6.3 (g)

— If further interference with an interference avoidance vector occurs

If the pocket shown in the Fig. 5.4.6.3 (h) is to be machined, if the number of blocks to read is 3, the end-point vector of block 1 and the end-point vector of block 2 are judged to interfere, and an attempt is made to calculate, as an interference avoidance vector, the intersection vector of the post-compensation path of block 1 and the post-compensation path of block 3. In this case, however, the end-point vector of block 3 that is to be calculated next further interferes with the previous interference avoidance vector. If a further interference occurs to the interference avoidance vector once created and output, the movement in the block will not be performed; an alarm will occur immediately before the block and the tool will stop.

Tool center path

Programmed path

Block 1

Block 2

Block 3

Block 5

The intersection vectors of blocks 3 and 4 further interfere.

Stopped

Block 4

Fig. 5.4.6.3 (h)

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 203 —

NOTE 1 For «If it is judged dangerous to avoid interference» and «If further interference

with an interference avoidance vector occurs», by setting bit 6 (NAA) of parameter No. 19607 appropriately, it is possible to suppress an alarm to continue machining. For «If no interference avoidance vector exists», however, it is not possible to avoid an alarm regardless of the setting of this parameter.

2 If a single block stop occurs during interference avoidance operation, and an operation is performed which differs from the original movement, such as manual intervention, MDI intervention, cutter or tool nose radius compensation value change, intersection calculation is performed with a new path. If such an operation is performed, therefore, an interference may occur again although interference avoidance has been performed once.

5.4.7 Cutter or Tool Nose Radius Compensation for Input from MDI

Explanation — MDI operation

During MDI operation, that is, if a program command is specified in MDI mode in the reset state to make a cycle start, intersection calculation is performed for compensation in the same way as in memory operation/DNC operation. Compensation is performed in the same way if a subprogram is called from program memory due to MDI operation.

Subprogram in program memory O9000 ; N1 G41 G17 G01 U10.0 V10.0 T0101 ; N2 V15.0 ; N3 U15.0 ; N4 V-15.0 ; N5 U-15.0 ; N6 G40 U-10.0 V-10.0 ; M99 ;

MDI command G00 X0 Y0 ; M98 P9000 ; M02 ;

Fig. 5.4.7 (a)

— MDI intervention

If MDI intervention is performed, that is, if a single block stop is performed to enter the automatic operation stop state in the middle of memory operation, DNC operation, and the like, and a program command is specified in MDI mode to make a cycle start, cutter compensation does not perform intersection calculation, retaining the last compensation vector before the intervention.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 204 —

MDI intervention

MDI intervention W30.0 ; U20.0 W20.0 ; U-20.0 W20.0 ;

MEM mode (G41) N2 U30.0 W10.0 ; N3 U-30.0 W10.0 ; N4 W40.0 ;

N2 N3 N4 Program command

Last compensation vector

Retained compensation vector

Fig. 5.4.7 (b)

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 205 —

5.5 VECTOR RETENTION (G38) In cutter or tool nose radius compensation, by specifying G38 in offset mode, it is possible to retain the compensation vector at the end position of the previous block, without performing intersection calculation.

Format (In offset mode) G38 IP_ ; IP :Value specified for axial movement

Explanation

— Vector retention By specifying the above command, a vector is created at the end point of the block immediately preceding the G38 block, vertical to that block. In the G38 block, the vertical vector output in the previous block is retained. G38 is a one-shot G code. With the next move command without a G38 command, the compensation vector is re-created.

Limitation — Mode

Specify G38 in either G00 or G01 mode. If it is specified in G02 or G03 (circular interpolation) mode, a radial error may occur at the start and end points.

— Start-up/cancel In start-up/cancel, the operation is as described in Subsections 5.4.2 and 5.4.4. Thus, G38 cannot be specified in the following blocks: 1) Start-up command (G41 or G42) block 2) Cancel command (G40) block 3) Block immediately preceding the cancel command (G40) block

Example

X axis

Z axis

(10.0, 0.0)

(15.0, 5.0)

Block N1 Offset vectorBlock N2

Block N3

Program command

Tool nose radiuscenter path

: : (In offset mode)N1 G38 X0.0 Z10.0 ;N2 G38 X5.0 Z15.0 ;N3 G38 X0.0 Z10.0 ;N4 Z20.0 ; : :

Fig. 5.5 (a)

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 206 —

5.6 CORNER CIRCULAR INTERPOLATION (G39) By specifying G39 in offset mode during cutter or tool nose radius compensation, corner circular interpolation can be performed. The radius of the corner circular interpolation equals the compensation value.

Format In offset mode G39 ;

or I_J_

G39 I_K_ ; J_K_

Explanation

— Corner circular interpolation When the command indicated above is specified, corner circular interpolation in which the radius equals compensation value can be performed. G41 or G42 preceding the command determines whether the arc is clockwise or counterclockwise. G39 is a one-shot G code.

— G39 without I, J, or K When G39; is programmed, the arc at the corner is formed so that the vector at the end point of the arc is perpendicular to the start point of the next block.

— G39 with I, J, and K When G39 is specified with I, J, and K, the arc at the corner is formed so that the vector at the end point of the arc is perpendicular to the vector defined by the I, J, and K values.

Limitation — Move command

In a block containing G39, no move command can be specified. Otherwise, an alarm will occur.

— Inner corner In an inner corner block, G39 cannot be specified. Otherwise, overcutting will occur.

— Corner arc velocity If a corner arc is specified with G39 in G00 mode, the corner arc block velocity will be that of the F command previously specified.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 207 —

Example — G39 without I, J, or K

:: (In offset mode)

N1 Z10.0 ;N2 G39 ;N3 X-10.0 ;

X axis

Z axis

(10.0, 0.0)

(10.0, -10.0)

Block N1 Offset vector

Block N2 (Corner arc)

Block N3

Programmed path

Tool nose radiuscenter path

Fig. 5.6 (a)

— G39 with I, J, and K

:: (In offset mode)

N1 Z10.0 ;N2 G39 I-1.0 K2.0 ;N3 X-10.0 Z20.0 ;

X axis

Z axis

Block N1Offset vector

Block N2 (Corner arc)

Block N3

Tool nose radiuscenter path

(I=-1.0, K=2.0)

(20.0, -10.0)

Programmedpath(10.0, 0.0)

Fig. 5.6 (b)

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 208 —

5.7 EXTENDED TOOL SELECTION

Overview In lathe system machines, tools are changed mainly with the following two methods: (1) With a turret holding multiple tools, tools are changed by turning the turret (T command). (2) With an automatic tool changer (ATC), tools are changed by using both cartridge indexing (T

command) and tool change (such as M06) commands. To support the tool change method explained in (2) above, the following tool selection specifications apply to this function: <1> Tool compensation by a T command is disabled. This means that the T command performs auxiliary

functions only. <2> Tool compensation is enabled by using a G code instead of the T command. In this case, the

following types of tool compensation are enabled: • Tool length compensation • Tool center point control (*1) • Tool offset (compensation equivalent to that of a T command in the case of turret rotation type)

*1 Options are required separately.

Format M06 T_ ; Change tool : Gxx D_ ; Tool compensation start : : G49 ; Tool compensation cancel

Gxx : Type of tool compensation G43/G44 : Tool length compensation G43.4 : Tool center point control type 1 G43.5 : Tool center point control type 2 G43.7 : Tool offset D_ : Tool compensation number

Explanation

— Selecting a tool change method Bit 3 (TCT) of parameter No. 5040 selects a tool change method. This changes the way for specifying tool compensation. This parameter setting has influence on the following range (Table 5.7 (a)):

Table 5.7 (a)

Bit 3 (TCT) of parameter No. 5040 = 0 (Turret type)

Bit 3 (TCT) of parameter No. 5040 = 1 (ATC type)

Operation of T command Auxiliary function (tool change) and tool

offset Auxiliary function (tool indexing) only

Tool compensation Specified with T code Specified with G43.7 D_ Compensation No. of tool

compensation Specified with T code Specified with D code

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 209 —

Bit 3 (TCT) of parameter No. 5040 = 0 (Turret type)

Bit 3 (TCT) of parameter No. 5040 = 1 (ATC type)

Compensation No. of tool nose radius compensation

Specified with T code Specified with D code

Command such as G43 Disabled (alarm) Enabled Compensation No. of G43, etc. — Specified with D code

— T command operation

(1) When bit 3 (TCT) of parameter No.5040 is 0 The T command performs an auxiliary function and tool offset. The code signal issued to the machine is the T command value except the last 1 to 3 digits. For example, suppose that the following command is issued when 2 is set in parameter No. 5028 (the number of digits comprising the offset number in the T code command): T0313 ; The T code signal sent to the machine indicates 03. The tool compensation number, indicated by the lowest 2 digits, is 13.

(2) When bit 3 (TCT) of parameter No. 5040 is 1 The T command performs an auxiliary function only. In this case, the code signal issued to the machine is the T command value. For example, suppose that the following is specified: T0313 ; The T code signal issued to the machine is 0313. The T code signal is not affected by the setting of parameter No. 5028 (the number of digits comprising the offset number in the T code command). The tool compensation number is not affected by this command.

— Tool offset

(1) When bit 3 (TCT) of parameter No.5040 is 0 The T command performs tool offset.

(2) When bit 3 (TCT) of parameter No.5040 is 1 The T command does not perform tool offset. To provide tool offset, specify G43.7 D_. Tool offset is performed in the same way as with the T command when bit 3 of parameter No. 5040 is 0.

— Compensation number of tool offset

(1) When bit 3 (TCT) of parameter No.5040 is 0 The lowest 1 to 3 digits of the T command are used. The number of digits is set in parameter No. 5028. When the tool geometry/wear offset option is provided, tool geometry offset and wear offset may also be assigned different compensation values by setting bit 1 (LGN) of parameter No. 5002. For details, refer to the description of the tool selection function in the Operator’s Manual (Common to Lath System/Machining Center System).

(2) When bit 3 (TCT) of parameter No.5040 is 1 Except that a compensation number is specified with a D command, the same operation as (1) above is performed.

— Compensation number of tool nose radius compensation Same as for tool offset described above.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 210 —

— Specification of G43, etc. (1) When bit 3 (TCT) of parameter No.5040 is 0

G codes of group 23 such as G43 cannot be specified. Specifying such a G code results in an alarm PS0366.

(2) When bit 3 (TCT) of parameter No.5040 is 1 G codes of group 23 such as G43 can be specified. The following G codes can be specified: G43/G44: Tool length compensation G43.4: Tool center point control type 1 G43.5: Tool center point control type 2 G43.7: Tool offset Specify a compensation number with D_. The D code is specified in the same way as for tool offset and tool nose radius compensation. The reverse meanings can be set for G43/G44 and G43.7 by setting bit 4 (TLG) of parameter No. 5040.

— Tool compensation memory

As the compensation amount used by the functions listed below, only the value set in Z on the tool compensation memory screen is used, Values such as values set for the X, R, and Y-axis offsets (optional function) are ignored. G43/G44: Tool length compensation G43.4: Tool center point control type 1 G43.5: Tool center point control type 2 As the compensation amount used in the following function, the values set for the X, Z, and Y-axis offsets (optional function) on the tool compensation memory screen are used: G43.7: Tool offset

Limitation — Switching between tool offset mode and another compensation mode

In the tool offset (G43.7) mode, a command such as a tool length compensation command (G43/G44, G43.1, G43.4, or G43.5) cannot be specified. Similarly, in a mode such as the tool length compensation mode (G43/G44, G43.1, G43.4, or G43.5), tool offset (G43.7) cannot be specified. Specifying such a command results in the alarm PS368. To switch between compensation types, specify G49 to cancel the current compensation mode before setting another compensation mode.

— Multiple repetitive canned cycle When a multiple repetitive canned cycle is executed with bit 3 (TCT) of parameter No. 5040 set to 1, note the following:

CAUTION 1 When a G71 to G76 command is specified in the Series 15 program format, a

value such as the depth of cut is specified with a D code. In this case, a D command specified after G71 to G76 is assumed to be the depth of cut. For example, suppose that the command shown below is specified. In this case, the D command <1> is assumed to be the tool compensation number, and the D command <2> is assumed to be the depth of cut. Example: D10 G71 P_Q_ U_ W_ D7000 F_ S_; <1> <2>

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 211 —

CAUTION 2 In the operation of G71 to G73, a G code such as G43 and a D command

specified in the finish figure blocks (the portion enclosed by the sequence numbers specified with P_ and Q_) are ignored, and the compensation amount set when the G71 to G73 block is specified becomes valid.

— Modifying the setting of bit 3 (TCT) of parameter No. 5040

WARNING

Before modifying the setting of this parameter, ensure that the offset is canceled. If the setting is modified with the offset applied, offset operation may be performed incorrectly after that, or alarm PS0368 may be issued.

5.8 AUTOMATIC TOOL OFFSET (G36, G37) When a tool is moved to the measurement position by execution of a command given to the CNC, the CNC automatically measures the difference between the current coordinate value and the coordinate value of the command measurement position and uses it as the offset value for the tool. When the tool has been already offset, it is moved to the measurement position with that offset value. If the CNC judges that further offset is needed after calculating the difference between the coordinate values of the measurement position and the commanded coordinate values, the current offset value is further offset. Refer to the instruction manuals of the machine tool builder for details.

Explanation — Coordinate system

When moving the tool to a position for measurement, the coordinate system must be set in advance. (The workpiece coordinate system for programming is used in common.)

— Movement to measurement position A movement to a measurement position is performed by specifying as follows in the MDI, or MEM mode : G36 Xxa ; or G37 Zza ; In this case, the measurement position should be xa or za (absolute programming). Execution of this command moves the tool at the rapid traverse rate toward the measurement position, lowers the feedrate halfway, then continues to move it until the approach end signal from the measuring instrument is issued. When the tool tip reaches the measurement position, the measuring instrument outputs the measurement position reach signal to the CNC which stops the tool.

— Offset The current tool offset value is further offset by the difference between the coordinate value (α or β) when the tool has reached the measurement position and the value of xa or za specified in G36Xxa or G37Zza. Offset value x = Current offset value x+(α-xa) Offset value z = Current offset value z+(β-za) xa : Programmed X-axis measurement point za : Programmed Z-axis measurement point These offset values can also be altered from the MDI keyboard.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 212 —

— Feedrate and alarm The tool, when moving from the stating position toward the measurement position predicted by xa or za in G36 or G37, is feed at the rapid traverse rate across area A. Then the tool stops at point T (xa-γ or za-γ) and moves at the measurement feedrate set by parameter No. 6241 across areas B, C, and D. If the approach end signal turns on during movement across area B, alarm is generated. If the approach end signal does not turn on before point V, and tool stops at point V and alarm PS0080 is generated.

Startingposition

Predicted measurement position

ε ε

TS (xs, zs)

X, Z

FR FPU V

A B C D

|xa-xs|. |za-zs|U (xa, za)

FR : Rapid traverse rateFP : Measurement feedrate (set by parameter(No.6241))γ : Parameters No.6251, No.6252ε : Parameters No.6254, No.6255

Fig. 5.8 (a) Feedrate and alarm

— G code

If bit 3 (G36) of parameter No. 3405 has been set to 1, G37.1 and G37.2 are used as the G codes for automatic tool compensation for the X- and Z-axes, respectively.

Example

800

100

380

300

Programmed zero point

Z-axis measurement position

X-axis measurement position

Tool number T01

Offset value Offset value (Before measurement) (After measurement) X 100.0 98.0 Z 0 4.0

Fig. 5.8 (b) G50 X760.0 Z1100.0 ; Programming of absolute zero point (Coordinate system setting) S01 M03 T0101 ; Specifies tool T1, offset number 1, and spindle revolution G36 X200.0 ; Moves to the measurement position If the tool has reached the measurement position at X198.0 ; since the correct

measurement position is 200 mm, the offset value is altered by 198.0-200.0=-2.0mm.

G00 X204.0 ; Refracts a little along the X axis. G37 Z800.0 ; Moves to the Z-axis measurement position. If the tool has reached the measurement position at X804.0, the offset value is

altered by 804.0-800.0=4.0mm.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 213 —

T0101 ; Further offsets by the difference. The new offset value becomes valid when the T code is specified again.

WARNING 1 Measurement speed(Fp), γ, and ε are set as parameters (Fp : No.6241, γ :

No.6251, ε : No.6254) by machine tool builder. ε must be positive numbers so that γ>ε.

2 Cancel the tool nose radius compensation before G36, G37. 3 A delay or variation in detection of the measurement position arrival signal is 0 to

2 msec on the CNC side excluding the PMC side (0.1 msec or less for high-speed measurement position arrival signal input (optional)). Therefore, the measurement error is the sum of 2 msec and a delay or variation (including a delay or variation on the receiver side) in propagation of the measurement position arrival signal on the PMC side, multiplied by the feedrate set in parameter No. 6241.

4 A delay or variation in time after detection of the measurement position arrival signal until a feed stops is 0 to 8 msec. To calculate the amount of overrun, further consider a delay in acceleration/deceleration, servo delay, and delay on the PMC side.

5 When a manual movement is inserted into a movement at a measurement feedrate, return the tool to the position before the inserted manual movement for restart.

6 When using the optional tool nose radius compensation function, the tool offset amount is determined considering the value of tool nose R. Make sure that tool nose radius value is set correctly.

(Condition under which the tool-nose radius compensation is considered) For the X-axis (first axis of the basic three axes) : TIP=0/5/7 For the Z-axis (third axis of the basic three axes) : TIP=0/6/8 For the Y-axis (second axis of the basic three axes) : TIP=0

Actual m

ovement

Movem

ent considering

toolnose radius value

Tool noseradiusvalue

Measurementposition

The tool actually moves from point A to point B, but the tool offset value is determined assuming that the tool moves to point C considering the tool nose radius value.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 214 —

NOTE 1 When there is no T code command before G36 or G37, alarm PS0081 is

generated. 2 When a T code is specified in the same block as G36 or G37, alarm PS0082 is

generated.

5.9 COORDINATE SYSTEM ROTATION (G68.1, G69.1) With the coordinate system rotation function, it is possible to rotate a figure specified in a program. For example, a program that produces patterns of a figure rotated at increasingly larger angles can be created as a pair of subprograms, one of which defines a figure, the other of which calls the figure definition subprogram by specifying rotation. This method is useful for reducing the program development time and the size of the program.

Rotationcenter

Rotation angle

Fig. 5.9 (a)

Format G17 G18 G68.1 α_ β_ R_ ; Starts rotating the coordinate system G19 : Coordinate system rotation mode : (the coordinates are rotated) G69.1 Cancels coordinate system rotation

G17 (G18 or G19) : Selects a plane where the figure to be rotated is α, β : Specify two coordinates (from among X, Y, and Z) of the rotation center that match

G17, G18, and G19. The values specified as the coordinates of the rotation center must always be absolute values.

R: Specifies the rotation angle as an absolute value. Counterclockwise rotation is assumed to be positive. However, setting bit 0 (RIN) of parameter No. 5400 enables the use of an incremental value. Incremental units of the angle: 0.001 degrees Specifiable range: -360,000 to +360,000

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 215 —

Rotation angle R (incremental value)Rotationcenter

(α, β)

Rotation angle R (absolute value)

Fig. 5.9 (b)

Explanation

— Plane selection G code, G17, G18, or G19 Plane selection G code (G17, G18, or G19) can be specified in a block ahead of the coordinate system rotation G code (G68.1). Do not specify G17, G18, or G19 in coordinate system rotation mode.

— Rotation center If the rotation center (α_, β_) is not specified, the location of the tool when G68.1 is issued is assumed as the rotation center.

— Rotation angle command If the rotation angle command (R_) is not specified, the value specified in parameter No. 5410 is used as the rotation angle. To specify angular displacement (R_) in 0.00001 degrees (one hundred-thousandth), set bit 0 (FRD) of parameter No. 11630 to 1. In this case, angular displacement R is specified within the range of -36000000 to 36000000.

— Coordinate rotation cancel The coordinate rotation cancel G code (G69.1) can be specified in the same block as other commands.

— Tool compensation Tool compensation, such as tool offset or tool nose radius compensation, is processed after coordinate system rotation is performed for a program defining a figure. G68.1 can be used in either G00 or G01 mode.

Limitation — Reference position return

A reference position return command G27, G28, G29, or G30 can be issued only in G69.1 mode.

— Changes to coordinates Do not attempt to change coordinates in G68.1 mode (commands such as G50, G54 to G59, and the tool offset command).

— Canned cycles Coordinate system rotation cannot be used in simple canned cycles, multiple repetitive canned cycles, or canned drilling cycles.

— Incremental command Always use absolute values in a move command that immediately follows the coordinate system rotation command (G68.1) or coordinate rotation cancel command (G69.1). Specifying an incremental value results in the move command failing to operate normally.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 216 —

— Note on the specification of one axis in coordinate system rotation With the parameter below, a move position in the case where one axis is specified in the absolute mode can selected. If two axes are specified, a movement is made to the same position, regardless of the setting of the parameter. Bit 5 (AX1) of parameter No. 11600 If one axis is specified in the absolute mode when the coordinate system rotation mode is set:

0: The specified position is first calculated in the coordinate system before rotation then the coordinate system is rotated.

1: The coordinate system is first rotated then a movement is made to the specified position in the rotated coordinate system. (FS16i/18i/21i-compatible specification)

This parameter changes the handling of coordinates on axes not specified, so that a position to be reached by movement changes.

(Example) G90 G0 X0 Y0 G01 X10. Y10. F6000 G68.1 X0 Y0 R45……..Specifies coordinate system rotation. Y14.142……………………Specifies one axis ….(1) G69.1 When bit 5 (AX1) of parameter No. 11600 = 0: The specified position is calculated in the coordinate system (XY) before rotation then the

coordinate system is rotated. So, with the specification of (1), the position on the unspecified X axis is X10, and the specified position is (X10,Y14.142). Next, a movement is made to the move position (X-2.929,Y17.071) obtained by 45° rotation.

Coordinates before coordinate system rotation is specified : X10,Y10

45°

Move position : X-2.929,Y17.071

●

Specified position : X10,Y14.142

Tool path

Fig. 5.9 (c)

When bit 5 (AX1) of parameter No. 11600 = 1: With the specification of (1), coordinates (X10,Y10) before coordinate system rotation are converted

to coordinates (X’14.142,Y’0) in the coordinate system (X’Y’) obtained by 45° rotation. Next, a movement is made to the specified position (X’14.142,Y’14.142), that is, the move position (X0,Y20).

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 217 —

Coordinates in rotated coordinate system : X’14.142,Y’0

Coordinates before coordinatesystem rotation is specified : X10,Y10

45° X

X’

Y’ ●

Specified position : X’14.142,Y’14.142 Move position : X0,Y20

Conversion

Tool path

Fig. 5.9 (d)

— Tool offset

When tool offset with coordinate system shift is enabled (when bit 2 (LWT) of parameter No. 5002 is set to 1 or bit 4 (LGT) of parameter No. 5002 is set to 0, if tool offset is specified in the coordinate system rotation mode, alarm PS0509 is issued. When bit 6 (EVO) of parameter No. 5001 is set to 1, if the tool offset value is changed, the same alarm is issued.

Example — Tool nose radius compensation and coordinate system rotation

G68.1 and G69.1 can be specified during tool nose radius compensation, provided that the coordinate system rotation plane coincides with the tool nose radius compensation plane. N1 G50 X0 Z0 G69.1 G01 ; N2 G42 X1000 Z1000 F1000 T0101 ; N3 G68 R-30000 ; N4 Z3000 ; N5 G03 U1000 R1000 ; N6 G01 Z1000 ; N7 U-1000 ; N8 G69.1 G40 X0 Z0 ;

Program before rotation

Program after rotation

30°

Tool path

(0, 0)

Fig. 5.9 (e)

— Repetitive coordinate system rotation

Coordinate system rotation can be repeated by calling a registered subprogram more than once, but with increasingly greater rotation angles.

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 218 —

Set bit 0 (RIN) of parameter No. 5400 to 1 to specify the rotation angle as being incremental. (G code A, radius programming along the X-axis) G50 X0 Z0 G18 ; G01 F200 T0101 ; M98 P2100 ; M98 P2200 L7 ; G00 X0 Z0 M30 ; O2200 ; G68.1 X0 Z0 R45.0 ; G90 M98 P2100 ; M99 ; O2100 ; G01 G42 X-10.0 Z0 ; X-10.0 Z4.142 ; X-7.071 Z7.071 ; G40 M99 ;

Programmed tool path

Tool path with an offset

(0, 0)

(0, -10.0)

Subprogram

Fig. 5.9 (f)

5.10 ACTIVE OFFSET VALUE CHANGE FUNCTION BASED ON MANUAL FEED

Overview When rough machining/semifinish machining is to be performed using a single tool, you may make a fine adjustment of a tool offset value. Moreover, at setup time, you may want to make a fine adjustment of a workpiece origin offset once set. With this function, a travel distance moved on an axis by manual feed is automatically added to the workpiece coordinate system or the currently valid offset number among the specified offset values (tool offset value/workpiece origin offset) to make a offset value change.

Explanation — Active offset value change mode

The active offset value change mode is set using the active offset value change mode signal. In this mode, a travel distance moved on an axis by manual feed is automatically added to the workpiece coordinate system or the currently valid offset number among the specified offset values (tool offset value/workpiece origin offset). The types of manual feed usable to make an offset value change in this mode are manual handle feed, incremental feed, and jog feed.

CAUTION 1 When a movement is being made on an axis for which an offset value is to be

changed, do not set the active offset value change mode. 2 In the active offset value change mode, do not reset the relative coordinate to 0

or preset the relative coordinate to a specified value.

— Specifying an offset value to be changed Specify a tool offset value/workpiece origin offset with the active offset selection signal. A method of axis selection for tool offset value change operation can be selected with bit 1 (ATP) of parameter No. 5041. In the active offset value change mode, an offset value selected is indicated by blinking display in the state display area on the screen as follows:

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 219 —

Table 5.10 (a) When changing the tool offset value for an axis on which a movement is made (parameter ATP=0)

Offset value selected State display Tool offset value TOFS

Workpiece origin offset WZR

Table 5.10 (b) When changing the tool offset value for an axis selected by the signal (parameter ATP=1) Offset value selected State display X-axis tool offset value OFSX Z-axis tool offset value OFSZ Y-axis tool offset value OFSY Workpiece origin offset WZR

CAUTION

When a movement is being made on an axis for which an offset value is to be changed in the active offset value change mode, do not change the specification of the offset value to be changed.

NOTE To change the tool offset value for the Y-axis, the option for Y-axis offset is

required.

— Changing a tool offset value The tool offset value with the offset number corresponding to an T code specified in automatic operation is changed. If there is no currently valid tool offset value as in a case where no T code is specified after a cycle start, tool offset value change is made even when a movement is made on an axis by manual feed. By making a movement on a basic axis (X, Z, or Y), a tool offset value change can be made. With a movement on a rotation axis, no tool offset value change can be made. While a tool offset value is being changed, a movement by manual feed can be made on one axis only.

Example — Specified T code: T0110 — Value set with offset number 10: 54.700 mm — Travel distance on the Z-axis by manual feed: -2.583 mm In this example, the Z-axis value for tool offset value number 10 is: 54.700+(-2.583) = 52.117 mm

CAUTION

When bit 1 (ATP) of parameter No. 5041 is set to 0, a tool offset value change can be made by making a movement on any of the basic axes. When an offset value change for an axis is undesirable, interlock the axis.

NOTE A changed tool offset value is handled according to bit 6 (EVO) of parameter No.

5001 and bit 6 (AON) of parameter No. 5041.

— Changing a workpiece origin offset value The workpiece origin offset of the workpiece coordinate system corresponding to a G code from G54 to G59 or from G54.1 P1 to P48 (300) specified during automatic operation is changed on an axis-by-axis basis. A valid workpiece coordinate system exists at all times. So, when a movement is made on an axis by manual feed, the workpiece origin offset of the workpiece coordinate system is changed without fail. This change can be made by a movement on an arbitrary axis, which may be a linear axis or a rotation

5.COMPENSATION FUNCTION PROGRAMMING B-64484EN-1/02

— 220 —

axis. While a workpiece origin offset change is being made, movements can be made on multiple axes by manual feed.

Example — Specified workpiece coordinate system : G56 — Workpiece origin offset of G56 (X axis) : 50.000 — Workpiece origin offset of G56 (Z axis) : 5.000 — Workpiece origin offset of G56 (C axis) : 180.000 — Workpiece origin offset of G56 (Y axis) : -60.000 — Travel distance on the X axis by manual feed : -10.000mm — Travel distance on the Z axis by manual feed : 10.000mm — Travel distance on the C axis by manual feed : 90.000deg — Travel distance on the Y axis by manual feed : -5.000mm In this example, the workpiece origin offsets of G56 are as follows:

— X axis : 50.000+(-10.000) = 40.000 — Z axis : 5.000+10.000 = 15.000 — C axis : 180.000+90.000 = 270.000 — Y axis : -60.000+(-5.000) = -65.000

— Presetting the relative position indication

By setting bit 5 (APL) of parameter No. 3115 to 1, the relative position indication (counter) can be automatically preset to 0 when the active offset value change mode is selected. In this case, the changed offset value can be restored to the original value by returning the relative position indication (counter) to 0 by manual feed.

— Emergency stop, servo alarm If an emergency stop occurs, a servo alarm is issued, or servo excitation is turned off, an offset value change is made also for a travel distance on an axis moved by follow-up in the active offset value change mode.

NOTE If a tool offset value is selected as an offset value to be changed, no offset value

change is made for a travel distance on a rotation axis moved by follow-up.

Limitation — Manual operation that cannot change an active offset value

In a mode other than the manual handle feed mode/incremental feed mode/jog feed mode, no active offset value can be changed. Moreover, no active offset value can be changed in the manual reference position return mode. Even in the modes mentioned above, do not change an active offset value in the following operations: • 3-dimensional manual feed • Manual numerical command • PMC axis control

— Axis that disables an active offset value from being changed With a rotation axis, no tool offset value can be changed using this function.

B-64484EN-1/02 PROGRAMMING 5.COMPENSATION FUNCTION

— 221 —

— Offset values that cannot be changed with the active offset value change function

With this function, a tool-noose radius compensation value, B-axis offset value, and second geometry offset value cannot be changed.

PROGRAMMING B-64484EN-1/02

— 222 —

6. MEMORY OPERATION USING Series 15 FORMAT

6 MEMORY OPERATION USING Series 15 FORMAT

By setting the setting-related parameter (bit 1 of parameter No. 0001), a program created in the Series 15 program format can be registered in memory for memory operation. Registration to memory and memory operation are possible for the functions which use the same tape format as that for the Series 15 as well as for the following functions which use a different program format: • Subprogram calling • Canned cycle • Multiple repetitive canned cycle • Canned cycle for drilling

NOTE Registration to memory and memory operation are possible only for the

functions available in this CNC. Chapter 6, «MEMORY OPERATION BY Series 15 FORMAT», consists of the following sections: 6.1 ADDRESSES AND SPECIFIABLE VALUE RANGE FOR SERIES 15 PROGRAM FORMAT.222 6.2 SUBPROGRAM CALLING……………………………………………………………………………………………….222 6.3 CANNED CYCLE …………………………………………………………………………………………………………….223 6.4 MULTIPLE REPETITIVE CANNED CYCLE……………………………………………………………………..240 6.5 CANNED CYCLE FOR DRILLING …………………………………………………………………………………..276

6.1 ADDRESSES AND SPECIFIABLE VALUE RANGE FOR Series 15 PROGRAM FORMAT

Some addresses which cannot be used for the this CNC can be used in the Series 15 program format. The specifiable value range for the Series 15 program format is basically the same as that for the this CNC. Sections II-6.2 to II-6.5 describe the addresses with a different specifiable value range. If a value out of the specifiable value range is specified, an alarm is issued.

6.2 SUBPROGRAM CALLING

Format M98 Pxxxx Lyyyy ;

P : Subprogram number L : Repetition count

Explanation

— Address Address L cannot be used in this CNC tape format but can be used in the Series 15 format. (When the custom macro option is provided, address L can be used regardless of whether the format is Series 15 or not, however.)

— Subprogram number The specifiable value range is the same as that for this CNC (1 to 9999). If a value of more than five digits is specified, the last four digits are assumed as the subprogram number.

B-64484EN-1/02 PROGRAMMING

— 223 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

— Repetition count

The repetition count L can be specified in the range from 1 to 9999. If no repetition count is specified, 1 is assumed.

6.3 CANNED CYCLE

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

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

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

2 A canned cycle can be performed on any plane (including parallel axes for plane definition). When G code system A is used, however, U, V, and W cannot be set as a parallel axis.

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

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

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

PROGRAMMING B-64484EN-1/02

— 224 —

6. MEMORY OPERATION USING Series 15 FORMAT

6.3.1 Outer Diameter/Internal Diameter Cutting Cycle (G90) This cycle performs straight or taper cutting in the direction of the length.

6.3.1.1 Straight cutting cycle

Format G90X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A’ in the Fig. 6.3.1.1 (a)) in the direction of the length

U_,W_ : Travel distance to the cutting end point (point A’ in the Fig. 6.3.1.1 (a)) in the direction of the length

F_ : Cutting feedrate

X/2

X axis

Z axis

2(F)3(F) 1(R)

4(R)

Z W

U/2A’

(R)….Rapid traverse(F) ….Cutting feed

Fig. 6.3.1.1 (a) Straight cutting cycle

Explanation

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

the plane (specified X-coordinate for the ZX plane) in rapid traverse. (2) Operation 2 moves the tool to the specified coordinate of the first axis on the plane (specified

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

(3) Operation 3 moves the tool to the start coordinate of the second axis on the plane (start X-coordinate for the ZX plane) in cutting feed.

(4) Operation 4 moves the tool to the start coordinate of the first axis on the plane (start Z-coordinate for the ZX plane) in rapid traverse. (The tool returns to the start point (A).)

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

cycle start button once.

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

B-64484EN-1/02 PROGRAMMING

— 225 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

6.3.1.2 Taper cutting cycle

Format ZpXp-plane G90 X(U)_ Z(W)_ I_ F_ ; YpZp-plane G90 Y(V)_ Z(W)_ K_ F_ ; XpYp-plane G90 X(U)_ Y(V)_ J_ F_ ;

X_,Y_,Z_ : Coordinates of the cutting end point (point A’ in the Fig. 6.3.1.2 (a)) in the direction of the length

U_,V_,W_ : Travel distance to the cutting end point (point A’ in the Fig. 6.3.1.2 (a)) in the direction of the length

I_,J_,K_ : Taper amount (I in the figure below) F_ : Cutting feedrate

3(F)

X/2

4(R)

U/2 1(R)

Z axis

2(F) I

X axis

A’

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

Fig. 6.3.1.2 (a) Taper cutting cycle

Explanation

Address I, J, or K for specifying a taper varies with the plane selected. 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 I, J, or K). For the cycle in the figure above, a minus sign is added to the taper amount.

NOTE The increment system of address I, J, or K for specifying a taper depends on the

increment system for the reference axis. Specify a radius value at I, J, or K.

PROGRAMMING B-64484EN-1/02

— 226 —

6. MEMORY OPERATION USING Series 15 FORMAT

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

cycle start button once.

— Relationship between the sign of the taper amount and tool path The tool path is determined according to the relationship between the sign of the taper amount (address I, J, or K) and the cutting end point in the direction of the length in the absolute or incremental programming as Table 6.3.1.2 (a).

Table 6.3.1.2 (a) Outer diameter machining Internal diameter machining

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

U/2 3(F)

4(R)

1(R)

2(F)W

U/2 3(F)

4(R)

1(R)

2(F)

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

at |I|≤|U/2| 4. U > 0, W < 0, I < 0

at |I|≤|U/2|

U/2 3(F)

4(R)

1(R)

2(F)

U/2 3(F)

4(R)

1(R)

2(F)

— Canceling the mode

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

6.3.2 Threading Cycle (G92)

6.3.2.1 Straight threading cycle

Format G92 X(U)_Z(W)_F_Q_;

X_,Z_ : Coordinates of the cutting end point (point A’ in the Fig. 6.3.2.1 (a)) in the direction of the length

U_,W_ : Travel distance to the cutting end point (point A’ in the Fig. 6.3.2.1 (a)) in the direction of the length

Q_ : Angle for shifting the threading start angle (Increment: 0.001 degrees, Valid setting range: 0 to 360 degrees) F_ : Thread lead (L in the Fig. 6.3.2.1 (a))

B-64484EN-1/02 PROGRAMMING

— 227 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

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.) r

Approx. 45°

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

A’

U/2

Fig. 6.3.2.1 (a) Straight threading

Explanation

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

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

the plane (specified X-coordinate for the ZX plane) in rapid traverse. (2) Operation 2 moves the tool to the specified coordinate of the first axis on the plane (specified

for the ZX plane) in rapid traverse. (Retraction after chamfering) (4) Operation 4 moves the tool to the start coordinate of the first axis on the plane (start Z-coordinate for

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

CAUTION Notes on this threading are the same as in threading in G32. However, a stop by feed hold is as follows; Stop after completion of path 3 of

threading cycle.

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

cycle start button once.

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

— Acceleration/deceleration for threading after interpolation Acceleration/deceleration for threading after interpolation 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.

PROGRAMMING B-64484EN-1/02

— 228 —

6. MEMORY OPERATION USING Series 15 FORMAT

— Time constant and FL feedrate for threading

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

NOTE Common parameters for specifying the amount and angle of thread chamfering

are used for this cycle and threading cycle with G76.

— Retraction after chamfering The Table 6.3.2.1 (a) lists the feedrate, type of acceleration/deceleration after interpolation, and time

constant of retraction after chamfering.

Table 6.3.2.1 (a) Bit 3 (CFR) of

parameter No. 1611 Parameter No.

1466 Description

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

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

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

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

— Shifting the start angle Address Q can be used to shift the threading start angle. The start angle (Q) increment is 0.001 degrees and the valid setting range is between 0 and 360

degrees. No decimal point can be specified.

— Feed hold in a threading cycle When the threading cycle retract function is not used, the machine stops at the end point of retraction

after chamfering (end point of operation 3) by feed hold applied during threading.

B-64484EN-1/02 PROGRAMMING

— 229 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

— Threading cycle retract When the «threading cycle retract» optional function is used, feed hold may be applied during

threading (operation 2). In this case, the tool immediately retracts with chamfering and returns to the start point on the second axis (X-axis), then the first axis (Z-axis) on the plane.

Feed hold is effected here.

Start point

Ordinary cycle

Rapid traverse

Motion at feed hold

X axis

Z axis

Cutting feed

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

CAUTION Another feed hold cannot be made during retreat.

— Inch threading

Inch threading specified with address E is allowed.

6.3.2.2 Taper threading cycle

Format ZpXp-plane G92 X(U)_ Z(W)_ I_ F_ Q_ ; YpZp-plane G92 Y(V)_ Z(W)_ K_ F_ Q_ ; XpYp-plane G92 X(U)_ Y(V)_ J_ F_ Q_ ;

X_,Y_,Z_ : Coordinates of the cutting end point (point A’ in the Fig. 6.3.2.2 (a)) in the direction of the length

U_,V_,W_ : Travel distance to the cutting end point (point A’ in the Fig. 6.3.2.2 (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) I_,J_,K : Taper amount (I in the figure below) F_ : Thread lead (L in the Fig. 6.3.2.2 (a))

PROGRAMMING B-64484EN-1/02

— 230 —

6. MEMORY OPERATION USING Series 15 FORMAT

Detailed chamfered thread

1(R)

Z axis

3(R)

4(R)

2(F)

U/2

X/2I

X axis

Approx. 45°

(The chamfered angle in the left figureis 45 degrees or less because of thedelay in the servo system.)

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

A’

Fig. 6.3.2.2 (a) Taper threading cycle

Explanation

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

NOTE The increment system of address I, J, or K for specifying a taper depends on the

increment system for the reference axis. Specify a radius value at I, J, or K.

taper amount to the specified coordinate of the second axis on the plane (specified X-coordinate for the ZX plane) in rapid traverse.

Operations 2, 3, and 4 after operation 1 are the same as for a straight threading cycle.

CAUTION Notes on this threading are the same as in threading in G32. However, a stop by feed hold is as follows; Stop after completion of path 3 of

threading cycle.

B-64484EN-1/02 PROGRAMMING

— 231 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

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

cycle start button once.

— Relationship between the sign of the taper amount and tool path The tool path is determined according to the relationship between the sign of the taper amount

(address I, J, or K) and the cutting end point in the direction of the length in the absolute or incremental programming as Table 6.3.2.2 (a).

Table 6.3.2.2 (a)

Outer diameter machining Internal diameter machining 1. U < 0, W < 0, I < 0 2. U > 0, W < 0, I > 0

U/2 3(F)

4(R)

1(R)

2(F)W

U/2 3(F)

4(R)

1(R)

2(F)

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

at |I|≤|U/2| 4. U > 0, W < 0, I < 0

at |I|≤|U/2|

U/2 3(F)

4(R)

1(R)

2(F)

U/2 3(F)

4(R)

1(R)

2(F)

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

— Acceleration/deceleration for threading after interpolation — Time constant and FL feedrate for threading — Thread chamfering — Retraction after chamfering — Shifting the start angle — Threading cycle retract — Inch threading

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

PROGRAMMING B-64484EN-1/02

— 232 —

6. MEMORY OPERATION USING Series 15 FORMAT

6.3.3 End Face Turning Cycle (G94)

6.3.3.1 Face cutting cycle

Format G94 X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A’ in the Fig. 6.3.3.1 (a)) in the direction of the end face

U_,W_ : Travel distance to the cutting end point (point A’ in the Fig. 6.3.3.1 (a)) in the direction of the end face

F_ : Cutting feedrate

X axis

4(R )

X/2

3(F)

Z axis

1(R )

2(F)

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

U /2

A ’

Fig. 6.3.3.1 (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).)

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

cycle start button once.

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

B-64484EN-1/02 PROGRAMMING

— 233 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

6.3.3.2 Taper cutting cycle

Format ZpXp-plane G94 X(U)_ Z(W)_ K _ F_ ; YpZp-plane G94 Y(V)_ Z(W)_ J _ F_ ; XpYp-plane G94 X(U)_ Y(V)_ I _ F_ ;

X_,Y_,Z_ : Coordinates of the cutting end point (point A’ in the Fig. 6.3.3.2 (a)) in the direction of the end face

U_,V_,W_ : Travel distance to the cutting end point (point A’ in the Fig. 6.3.3.2 (a)) in the direction of the end face

I_,J_,K_ : Taper amount (K in the Fig. 6.3.3.2 (a)) 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’

Fig. 6.3.3.2 (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 end face and the sign of the taper amount (address I, J, or K). For the cycle in the figure above, a minus sign is added to the taper amount.

NOTE The increment system of address I, J, or K for specifying a taper depends on the

increment system for the reference axis. Specify a radius value at I, J, or K.

PROGRAMMING B-64484EN-1/02

— 234 —

6. MEMORY OPERATION USING Series 15 FORMAT

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

cycle start button once.

— Relationship between the sign of the taper amount and tool path The tool path is determined according to the relationship between the sign of the taper amount (address I, J, or K) and the cutting end point in the direction of the end face in the absolute or incremental programming as Table 6.3.3.2 (a).

Table 6.3.3.2 (a) Outer diameter machining Internal diameter machining

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

X1(R)

U/2

3(F)

4(R)2(F)

WKZ

U/2

3(F)

4(R)2(F)

1(R)

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

at |K|≤|W| 4. U > 0, W < 0, K < 0

at |K|≤|W|

U/2

3(F)

4(R)2(F)

1(R)

X W

U/2

3(F)

4(R)2(F)

1(R)

— Canceling the mode

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

B-64484EN-1/02 PROGRAMMING

— 235 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

6.3.4 How to Use Canned Cycles An appropriate canned cycle is selected according to the shape of the material and the shape of the product. — Straight cutting cycle (G90)

Shape of product

Shape of material

— Taper cutting cycle (G90)

Shape of product

Shape of material

— Face cutting cycle (G94)

Shape of product

Shape of material

PROGRAMMING B-64484EN-1/02

— 236 —

6. MEMORY OPERATION USING Series 15 FORMAT

— Face taper cutting cycle (G94)

Shape of product

Shape of material

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

Outer diameter/internal diameter cutting cycle (G90) Tool nose radius center path Offset direction

Whole tool nose

Tool nose radius center path

Programmed path

5 7

1 6 2

Wholetool nose

Whole tool nose

End face cutting cycle (G94)

Tool nose radius center path Offset direction

Whole tool nose

Tool nose radius center path

Programmed path

5 7

1 6 2

Wholetool nose

Whole tool nose

B-64484EN-1/02 PROGRAMMING

— 237 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

Threading cycle (G92)

Tool nose radius compensation cannot be applied.

Differences between this CNC and the Series 16i/18i/21i NOTE This CNC is the same as the 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 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, refer to «Series 16i/18i/21i Operator’s Manual.»

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

G90 G94

4,8,3

5,0,7

1,6,2

4,5,1 8,0,6

3,7,2

Wholetool nose

Tool nose radius center path

Programmed path

5 7

1 62

5 7

1 62

4,5,1 8,0,6

3,7,2

Wholetool nose

4,8,3

5,0,7

1,6,2

Programmed path

Tool nose radius center path

6.3.6 Restrictions on Canned Cycles

Limitation — Modal

PROGRAMMING B-64484EN-1/02

— 238 —

6. MEMORY OPERATION USING Series 15 FORMAT

Example

Workpiece

161284

66X axis

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

N003 T0101;

N010 G90 X20.0 Z10.0 F0.2;

N011 G00 T0202; ← Cancels the canned cycle mode.

N012 G90 X20.5 Z10.0;

— Plane selection command

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

B-64484EN-1/02 PROGRAMMING

— 239 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

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.

1(R)

3(F)

4(R)2(F)

Manual intervention Cancellation

Example of G94

PROGRAMMING B-64484EN-1/02

— 240 —

6. MEMORY OPERATION USING Series 15 FORMAT

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

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

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

2 A multiple repetitive canned cycle can be performed on any plane (including parallel axes for plane definition). When G code system A is used, however, U, V, and W cannot be set as a parallel axis.

B-64484EN-1/02 PROGRAMMING

— 241 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

6.4.1 Stock Removal in Turning (G71) There are two types of stock removal in turning : Type I and II. To use type II, the «multiple repetitive canned cycle 2» optional function is required.

Format ZpXp plane

G71 P(ns) Q(nf) U(Δu) W(Δw) I(Δi) K(Δk) D(Δd) F(f ) S(s ) T(t ); N (ns) ;

…

N (nf) ;

The move command between A and B is specified in the blocks from sequence number ns to nf.

YpZp plane

G71 P(ns) Q(nf) V(Δw) W(Δu) J(Δk) K(Δi) D(Δd) F(f ) S(s ) T(t ); N (ns) ; … N (nf) ;

XpYp plane G71 P(ns) Q(nf) U(Δw) V(Δu) I(Δk) J(Δi) D(Δd) F(f ) S(s ) T(t ); N (ns) ; … N (nf) ;

Δd : Depth of cut The cutting direction depends on the direction AA’. ns : Sequence number of the first block for the program of finishing shape. nf : Sequence number of the last block for the program of finishing shape. Δu : Distance of the finishing allowance in the direction of the second axis on the plane

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

(Z-axis for the ZX plane) Δi : Distance of the finishing allowance of the roughing in the direction of the second

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

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

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

NOTE Even if pocket calculator type decimal point programming is specified (bit 0 (DPI)

of parameter No. 3401 = 1), the unit of address D is least input increment. In addition, when a decimal point is input in address D, the alarm PS0007 is issued.

Unit Diameter/radius programming Sign Decimal point input

Δd Depends on the increment system for the reference axis.

Radius programming Not

required Not allowed

PROGRAMMING B-64484EN-1/02

— 242 —

6. MEMORY OPERATION USING Series 15 FORMAT

Unit Diameter/radius programming Sign Decimal point input

Δu Depends on the increment system for the reference axis.

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

Required Allowed

Δw Depends on the increment system for the reference axis.

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

Required Allowed

Δi Depends on the increment system for the reference axis.

Radius programming Not

required Allowed

Δk Depends on the increment system for the reference axis.

Radius programming Not

required Allowed

(R)

(F)

Δu/2

Δd

A’

ΔW

Target figure

45° e

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

+Ze: Escaping amount (parameter No.5133)

Fig. 6.4.1 (a) Cutting path of an outer surface rough cutting cycle

without rough cutting finishing allowance (type I)

B (R)

(R)

(F)

Δu/2

Δd

A’

ΔW

Target figure

45° e

(F): Cutting feed

(R): Rapid

(R)

ΔK

Δi

e: Escaping amount (parameter No.5133) Fig. 6.4.1 (b) Cutting path of an outer surface rough cutting cycle

with rough cutting finishing allowance (type I)

B-64484EN-1/02 PROGRAMMING

— 243 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

Explanation — Operations

If a target figure passing through A, A’, and B in this order is given by the program, a workpiece is cut away by depth of cut Δd at a time. The machining path varies as follows depending on whether the rough machining finishing allowance is specified. (1) When the rough cutting finishing allowance is not specified

Cutting is performed by depth of cut Δd with finishing allowances Δu/2 and Δw left, and rough cutting as finishing is performed according to the target figure program after the last machining.

(2) When the rough cutting finishing allowance is specified Cutting is performed by depth of cut Δd with cutting allowances Δu/2+Δi and Δw+Δk left, and the tool returns to the start point (A) after the last cutting is performed. Then, rough machining as finishing is performed along the target figure to remove cutting allowances Δi and Δk.

Upon completion of rough machining as finishing, the block next to the sequence block specified by Q is executed.

NOTE 1 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.

2 When a constant surface speed control is provided, G96 or G97 command specified in the move command between points A and B are ineffective, and that specified in G71 block or the previous block is effective.

— Escaping amount (e)

The escaping amount (e) is set in parameter No. 5133.

No. Unit Diameter/radius programming Sign

5133 Depends on the increment system for the reference axis.

Radius programming Not required

— Target figure Patterns

Both linear andcircular interpolationare possible

A’

U(+)…W(+)

A’

U(+)…W(-)

A’

B A

U(-)…W(+)

A’

U(-)…W(-)

Fig. 6.4.1 (c) Four target figure patterns

PROGRAMMING B-64484EN-1/02

— 244 —

6. MEMORY OPERATION USING Series 15 FORMAT

Limitation

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

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

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

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

Start block In the start block in the program for a target figure (block with sequence number ns in which the path between A and A’ is specified), G00 or G01 must be specified. If it is not specified, alarm PS0065 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.

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

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

compensation is applied is checked. The following checks can also be made.

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

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

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

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

— Types I and II Selection of type I or II

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

Selecting type I or II

plane (Z-axis for the ZX plane).

B-64484EN-1/02 PROGRAMMING

— 245 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

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

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

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

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

plane) must be specified.

Example ZX plane G71 V10.0 R5.0 ; G71 P100 Q200….; N100 X(U)_ ; (Specifies only the second axis on the plane.) : ; : ; N200…………;

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

forming the plane (Z- and X-axes for the ZX plane). It must not have any pocket as shown in the Fig. 6.4.1 (d).

No pockets are allowed.

A’

Fig. 6.4.1 (d) Figure which does not show monotone increase or decrease (type I)

CAUTION

If a figure does not show monotone change along the first or second axis on the plane, alarm PS0064 or 0329 is issued. If the movement does not show monotone change, but is very small, and it can be determined that the movement is not dangerous, however, the permissible amount can be specified in parameters Nos. 5145 and 5146 to specify that the alarm is not issued in this case.

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

Escaping amount e (specified in the command or parameter No. 5133) 45°

Fig. 6.4.1 (e) Cutting in the direction of 45 degrees (type I)

(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. When the rough cutting finishing allowance is specified, however, rough cutting as finishing is performed.

PROGRAMMING B-64484EN-1/02

— 246 —

6. MEMORY OPERATION USING Series 15 FORMAT

— Type II

(F)

Δu/2

Δd

A’

ΔW

Target figure

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

(R)

Δd

(F)

(R)(R)

Fig. 6.4.1 (f) Cutting path in stock removal in turning (type II)

When the figure program for instructing a target figure passing through A, A’, and B in this order is specified, a workpiece is cut away by depth of cut Δd at a time. In type II, cutting is performed along the figure after rough cutting in the direction of the plane first axis (z-axis for the ZX plane). The machining path varies as follows depending on whether the rough machining finishing allowance is specified. (1) When the rough cutting finishing allowance is not specified

Cutting is performed by depth of cut Δd with finishing allowances Δu/2 and Δw left, and the tool returns to the start point (A) after the last cutting is performed (one pocket is assumed because Pn→Pm is parallel to the z-axis in the Fig. 6.4.1 (f), and the zone is cut). Then, rough machining as finishing is performed according to the finishing figure program with finishing allowances Δu/2 and Δw left.

Upon completion of rough machining as finishing, the block next to the sequence block specified by Q is executed. 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.

Example

ZX plane G71 V10.0 R5.0; G71 P100 Q200…….; N100 X(U)_ Z(W)_ ; (Specifies the two axes forming the plane.) : ; : ; N200…………;

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

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

B-64484EN-1/02 PROGRAMMING

— 247 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

1 2 3 10 . . .

+Z Fig. 6.4.1 (g) Figure having pockets (type II)

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

ZX plane), however. The following figure cannot be machined.

Monotone change is not observed along the Z-axis.

+Z Fig. 6.4.1 (h) Figure which cannot be machined (type II)

CAUTION

For a figure along which the tool moves backward along the first axis on the plane during cutting operation (including a vertex in an arc command), the cutting tool may contact the workpiece. For this reason, for a figure which does not show monotone change, alarm PS0064 or PS0329 is issued. If the movement does not show monotone change, but is very small, and it can be determined that the movement is not dangerous, however, the permissible amount can be specified in parameter No. 5145 to specify that the alarm is not issued in this case.

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

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

Fig. 6.4.1 (i) Figure which can be machined (type II) (3) After turning, the tool cuts the workpiece along its figure and escapes in cutting feed.

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

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

Escaping after cutting

Fig. 6.4.1 (j) Cutting along the workpiece figure (type II)

PROGRAMMING B-64484EN-1/02

— 248 —

6. MEMORY OPERATION USING Series 15 FORMAT

The escaping amount e after cutting is set in parameter No. 5133. When moving from the bottom, however, the tool escapes to the direction of 45 degrees.

e (specified in the command orparameter No. 5133) 45°

Bottom

Fig. 6.4.1 (k) 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

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

Depth of cut Δd

Start point

Escaping operation afterrough cutting

Escaping operation after rough cuttingas finishing

Fig. 6.4.1 (l) 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)

<1><2><3>

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

Fig. 6.4.1 (m) Rough cutting order in the case of monotone decrease (type II)

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

B-64484EN-1/02 PROGRAMMING

— 249 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

<3><2><1>

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

Fig. 6.4.1 (n) Rough cutting order in the case of monotone increase (type II) The path in rough cutting is as shown Fig. 6.4.1 (o).

28 30

2522

9 102

14 20

1319

5 1

611

1216

3132

Fig. 6.4.1 (o) Cutting path for multiple pockets (type II)

The Fig. 6.4.1 (p) shows how the tool moves after rough cutting for a pocket in detail.

22 21•

g Rapid traverse

Escaping fromthe bottom

Cutting feed

Fig. 6.4.1 (p) Details of motion after cutting for a pocket (type II)

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

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

PROGRAMMING B-64484EN-1/02

— 250 —

6. MEMORY OPERATION USING Series 15 FORMAT

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

allowance). Otherwise, the tool may dig into the wall on one side. 3 This CNC differs from the FANUC Series 16i/18i/21i in the path of cutting after

— Tool nose radius compensation

When using tool nose radius compensation, specify a tool nose radius compensation command (G41, G42) before a multiple repetitive canned cycle command (G70, G71, G72, G73) and specify the cancel command (G40) outside the programs (from the block specified with P to the block specified with Q) specifying a target finishing figure. If tool nose radius compensation is specified in the program specifying a target finishing figure, alarm PS0325, “UNAVAILABLE COMMAND IS IN SHAPE PROGRAM”, is issued. Program example G42;…………………………Specify this command before a multiple repetitive canned cycle command. G71P10Q20D1000 ; N10G00X0; : N20X50.; G40;…………………………Specify this command after the program specifying a target finishing figure. When this cycle is specified in the tool nose radius compensation mode, offset is temporarily canceled during movement to the start point. Start-up is performed in the first block. Offset is temporarily canceled again at the return to the cycle start point after termination of cycle operation. Start-up is performed again according to the next move command. This operation is shown in the Fig. 6.4.1 (q).

Cycle start point

Start-up

Offset cancel

Start-up

Offset cancel

Fig. 6.4.1 (q)

B-64484EN-1/02 PROGRAMMING

— 251 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

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

B A

A’

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

Position between A-A’ in which start-up is performed

Fig. 6.4.1 (r) Path when tool nose radius compensation is applied

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

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

B A

A’

Position between A-A’ in which start-up is performed

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

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

— Reducing the cycle time

PROGRAMMING B-64484EN-1/02

— 252 —

6. MEMORY OPERATION USING Series 15 FORMAT

For the type I command

+Z : Rapid traverse can be selected. : The mode specified in the start block is followed.

Operation 1

Operation 2

Previous turning point

Current turning point

For the type II command

Operation 1

Operation 2

Previous turning point

Current turning point

B-64484EN-1/02 PROGRAMMING

— 253 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

6.4.2 Stock Removal in Facing (G72) This cycle is the same as G71 except that cutting is performed by an operation parallel to the second axis on the plane (X-axis for the ZX plane).

Format ZpXp plane

G72 P(ns) Q(nf) U(Du) W(Dw) I(Di) K(Dk) D(Dd) F(f ) S(s ) T(t );

N (ns) ;

…

N (nf) ;

The move command between A and B is specified in the blocks from sequencenumber ns to nf.

YpZp plane G72 P(ns) Q(nf) V(Δw) W(Δu) J(Δk) K(Δi) D(Δd) F(f ) S(s ) T(t ); N (ns) ; … N (nf) ;

XpYp plane G72 P(ns) Q(nf) U(Δw) V(Δu) I(Δk) J(Δi) D(Δd) F(f ) S(s ) T(t ); N (ns) ; … N (nf) ;

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

(Z-axis for the ZX plane) Δi : Distance of the finishing allowance of the roughing in the direction of the second

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

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

F, S, or T function in this G72 block is effective.

NOTE Even if pocket calculator type decimal point programming is specified bit 0 (DPI)

of parameter No. 3401 = 1, the unit of address D is least input increment. In addition, when a decimal point is input in address D, the alarm PS0007, “ILLEGAL USE OF DECIMAL POINT” is issued.

PROGRAMMING B-64484EN-1/02

— 254 —

6. MEMORY OPERATION USING Series 15 FORMAT

Unit Diameter/radius programming Sign Decimal point input

Δd Depends on the increment system for the reference axis.

Radius programming Not required Not allowed

Δu Depends on the increment system for the reference axis.

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

Required Allowed

Δw Depends on the increment system for the reference axis.

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

Required Allowed

Δi Depends on the increment system for the reference axis.

Radius programming Not required Allowed

Δk Depends on the increment system for the reference axis.

Radius programming Not required Allowed

A’

Δu/2

Δd

Tool path (F)

(R)

45°

(R)

(F)

Δw

Target figure

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

e: Escaping amount (parameter No.5133)

Fig. 6.4.2 (a) Cutting path in stock removal in facing (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 Δd (depth of cut), with the finishing allowance specified by Δu/2 and Δw left.

NOTE 1 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.

2 When a constant surface speed control is provided, G96 or G97 command specified in the move command between points A and B are ineffective, and that specified in G72 block or the previous block is effective.

— Escaping amount (e)

The escaping amount (e) is set in parameter No. 5133.

B-64484EN-1/02 PROGRAMMING

— 255 —

6.MEMORY OPERATIONUSING Series 15 FORMAT

No. Unit Diameter/radius programming Sign

5133 Depends on the increment system for the reference axis.

Radius programming Not required

— Target figure Patterns

Both linear and circular interpolation are possible

+Z B

U(-)…W(+)…

A’

U(-)…W(-)…

A’

U(+)…W(+)…

A’

U(+)…W(-)…

A’

Fig. 6.4.2 (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 first and second axes on the plane.

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

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

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

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

compensation is applied is checked. The following checks can also be made.

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

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

PROGRAMMING B-64484EN-1/02

— 256 —

6. MEMORY OPERATION USING Series 15 FORMAT

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

Enabled when bit 2 (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. With type I, the tool escapes to the direction of 45 degrees. With type II, the tool cuts the workpiece along the target figure. When the target figure has no pockets, determine the desired escaping operation and select type I or II.