fanuc 16C, 160C, 18C, 180-C Operators Manual

Download

GE Fanuc Automation

Computer Numerical Control Products

Series 16 / 18 / 160 / 180 – Model C for Machining Center

Operator's Manual

B-62764EN/01 December 1995

Warnings, Cautions, and Notes as Used in this Publication

Warning notices are used in this publication to emphasize that hazardous voltages, currents, temperatures, or other conditions that could cause personal injury exist in this equipment or may be associated with its use.

In situations where inattention could cause either personal injury or damage to equipment, a Warning notice is used.

Caution notices are used where equipment might be damaged if care is not taken.

GFL-001

Warning

Caution

Note

Notes merely call attention to information that is especially significant to understanding and operating the equipment.

This document is based on information available at the time of its publication. While efforts have been made to be accurate, the information contained herein does not purport to cover all details or variations in hardware or software, nor to provide for every possible contingency in connection with installation, operation, or maintenance. Features may be described herein which are not present in all hardware and software systems. GE Fanuc Automation assumes no obligation of notice to holders of this document with respect to changes subsequently made.

GE Fanuc Automation makes no representation or warranty, expressed, implied, or statutory with respect to, and assumes no responsibility for the accuracy, completeness, sufficiency, or usefulness of the information contained herein. No warranties of merchantability or fitness for purpose shall apply.

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

1. DEFINITION OF WARNING, CAUTION, AND NOTE s–2. . . . . . . . . . . . . . . . . . . . . . . .

2. GENERAL WARNINGS AND CAUTIONS s–3. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3. WARNINGS AND CAUTIONS RELATED TO PROGRAMMING s–5. . . . . . . . . . . . . .

4. WARNINGS AND CAUTIONS RELATED TO HANDLING s–7. . . . . . . . . . . . . . . . . . . .

5. WARNINGS RELATED TO DAILY MAINTENANCE s–9. . . . . . . . . . . . . . . . . . . . . . . . .

s–1

SAFETY PRECAUTIONS

B–62764EN/01

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

CAUTION

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

NOTE

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

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

s–2

B–62764EN/01

SAFETY PRECAUTIONS

GENERAL WARNINGS AND CAUTIONS

WARNING

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.

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.

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.

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.

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.

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

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.

s–3

SAFETY PRECAUTIONS

B–62764EN/01

W ARNING

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.

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.

s–4

B–62764EN/01

SAFETY PRECAUTIONS

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 and programming manual carefully such that you are fully familiar with their contents.

WARNING

Coordinate system setting

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

Positioning by nonlinear interpolation

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

Function involving a rotation axis

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

Inch/metric conversion

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

Constant surface speed control

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

s–5

SAFETY PRECAUTIONS

W ARNING

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.

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.

Absolute/incremental mode

B–62764EN/01

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

Plane selection

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

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.

s–6

B–62764EN/01

SAFETY PRECAUTIONS

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 and programming manual carefully, such that you are fully familiar with their contents.

WARNING

Manual operation

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

Manual reference position return

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

Manual numeric command

When issuing a manual numeric command, determine the current position of the tool and workpiece, and ensure that the movement axis, direction, and command have been specified correctly, and that the entered values are valid. Attempting to operate the machine with an invalid command specified may damage the tool, the machine itself, the workpiece, or cause injury to the operator.

Manual handle feed

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

Disabled override

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

Origin/preset operation

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

s–7

SAFETY PRECAUTIONS

W ARNING

Workpiece coordinate system shift

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

Software operator’s panel and menu switches

Using the software operator’s panel and menu switches, in combination with the MDI panel, 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 panel keys are operated inadvertently, the machine may behave unexpectedly, possibly damaging the tool, the machine itself, the workpiece, or causing injury to the user.

B–62764EN/01

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.

10.

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.

11.

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.

12.

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.

13.

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.

s–8

B–62764EN/01

SAFETY PRECAUTIONS

WARNINGS RELATED TO DAILY MAINTENANCE

WARNING

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 fitted with an insulating cover). Touching the uncovered high–voltage circuits presents an extremely dangerous electric shock hazard.

and

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 CR T 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 maintenance section of the operator’s manual or programming manual for details of the battery replacement procedure.

s–9

SAFETY PRECAUTIONS

B–62764EN/01

W ARNING

Absolute pulse coder battery replacement

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 CR T 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 maintenance section of the operator’s manual or programming manual for details of the battery replacement procedure.

and

s–10

B–62764EN/01

SAFETY PRECAUTIONS

W ARNING

Fuse replacement

For some units, the chapter covering daily maintenance in the operator’s manual or programming manual describes the fuse replacement procedure. 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 Touching an uncovered high–voltage circuit presents an extremely dangerous electric shock hazard.

and fitted with an insulating cover).

s–1 1

B–62764EN/01

SAFETY PRECAUTIONS S–1. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

I. GENERAL

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

1.1 GENERAL FLOW OF OPERATION OF CNC MACHINE TOOL 5. . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.2 NOTES ON READING THIS MANUAL 7. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

II. PROGRAMMING

1. GENERAL 11. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.1 TOOL MOVEMENT ALONG WORKPIECE PARTS FIGURE–INTERPOLATION 12. . . . . . . . . . . .

1.2 FEED–FEED FUNCTION 14. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.3 PART DRAWING AND TOOL MOVEMENT 15. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.3.1 Reference Position (Machine–Specific Position) 15. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.3.2 Coordinate System on Part Drawing and Coordinate System Specified

by CNC – Coordinate System 16. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.3.3 How to Indicate Command Dimensions for Moving the Tool – Absolute,

Incremental Commands 19. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4 CUTTING SPEED – SPINDLE SPEED FUNCTION 20. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.5 SELECTION OF TOOL USED FOR VARIOUS MACHINING – TOOL FUNCTION 21. . . . . . . . . . .

1.6 COMMAND FOR MACHINE OPERATIONS – MISCELLANEOUS FUNCTION 22. . . . . . . . . . . . .

1.7 PROGRAM CONFIGURATION 23. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.8 TOOL FIGURE AND TOOL MOTION BY PROGRAM 26. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.9 TOOL MOVEMENT RANGE – STROKE 27. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2. CONTROLLED AXES 28. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1 CONTROLLED AXES 29. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.2 AXIS NAME 29. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3 INCREMENT SYSTEM 31. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4 MAXIMUM STROKE 32. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3. PREPARATORY FUNCTION (G FUNCTION) 33. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4. INTERPOLATION FUNCTIONS 38. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.1 POSITIONING (G00) 39. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.2 SINGLE DIRECTION POSITIONING (G60) 41. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.3 LINEAR INTERPOLATION (G01) 43. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.4 CIRCULAR INTERPOLATION (G02,G03) 45. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.5 HELICAL INTERPOLATION (G02,G03) 49. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.6 POLAR COORDINATE INTERPOLA TION (G12.1,G13.1) 50. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.7 CYLINDRICAL INTERPOLATION (G07.1) 54. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8 INVOLUTE INTERPOLATION (G02.2, G03.2) 57. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–1

TABLE OF CONTENTS

4.9 EXPONENTIAL INTERPOLATION (G02.3, G03.3) 63. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.10 SMOOTH INTERPOLATION (G05.1) 67. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.11 HYPOTHETICAL AXIS INTERPOLATION (G07) 71. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.12 THREAD CUTTING (G33) 73. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.13 SKIP FUNCTION(G31) 75. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.14 MULTISTAGE SKIP (G31) 77. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.15 HIGH SPEED SKIP SIGNAL (G31) 78. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.16 CONTINUOUS HIGH–SPEED SKIP FUNCTION (G31) 79. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–62764EN/01

5. FEED FUNCTIONS 80. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.1 GENERAL 81. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.2 RAPID TRAVERSE 83. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.3 CUTTING FEED 84. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4 CUTTING FEEDRATE CONTROL 89. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.1 Exact Stop (G09, G61) Cutting Mode (G64) Tapping Mode (G63) 90. . . . . . . . . . . . . . . . . . . . . . .

5.4.2 Automatic Override for Inner Corners (G62) 91. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.3 Internal Circular Cutting Feedrate Change 94. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.4 Automatic Corner Deceleration 95. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.5 DWELL (G04) 102. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6. REFERENCE POSITION 103. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7. FLOATING REFERENCE POSITION RETURN (G30.1) 108. . . . . . . . . . . . . . . . . . . . . . . .

8. COORDINATE SYSTEM 110. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1 MACHINE COORDINATE SYSTEM 11 1. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2 WORKPIECE COORDINATE SYSTEM 112. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2.1 Setting a Workpiece Coordinate System 112. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2.2 Selecting a Workpiece Coordinate System 113. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2.3 Changing Workpiece Coordinate System 114. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2.4 Workpiece Coordinate System Preset (G92.1) 117. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2.5 Adding Workpiece Coordinate Systems (G54.1 or G54) 119. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3 LOCAL COORDINATE SYSTEM 121. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4 PLANE SELECTION 123. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9. COORDINATE VALUE AND DIMENSION 124. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1 ABSOLUTE AND INCREMENTAL PROGRAMMING (G90, G91) 125. . . . . . . . . . . . . . . . . . . . . . . .

9.2 POLAR COORDINATE COMMAND (G15, G16) 126. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3 INCH/METRIC CONVERSION (G20,G21) 129. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4 DECIMAL POINT PROGRAMMING 130. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10. SPINDLE SPEED FUNCTION (S FUNCTION) 131. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.1 SPECIFYING THE SPINDLE SPEED WITH A CODE 132. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2 SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY (S5–DIGIT COMMAND) 132. . . . . . . . .

10.3 CONSTANT SURFACE SPEED CONTROL (G96, G97) 133. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.4 SPINDLE SPEED FLUCTUATION DETECTION FUNCTION (G25, G26) 136. . . . . . . . . . . . . . . . . .

c–2

B–62764EN/01

TABLE OF CONTENTS

11. TOOL FUNCTION (T FUNCTION) 139. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1 TOOL SELECTION FUNCTION 140. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2 TOOL LIFE MANAGEMENT FUNCTION 141. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.1 Tool Life Management Data 142. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.2 Register, Change and Delete of Tool Life Management Data 143. . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.3 Tool Life Management Command in a Machining Program 146. . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.4 Tool Life 149. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12. AUXILIARY FUNCTION 150. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.1 AUXILIARY FUNCTION (M FUNCTION) 151. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.2 MULTIPLE M COMMANDS IN A SINGLE BLOCK 152. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.3 M CODE GROUP CHECK FUNCTION 153. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.4 THE SECOND AUXILIARY FUNCTIONS (B CODES) 154. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13. PROGRAM CONFIGURATION 155. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1 PROGRAM COMPONENTS OTHER THAN PROGRAM SECTIONS 157. . . . . . . . . . . . . . . . . . . . .

13.2 PROGRAM SECTION CONFIGURATION 160. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.3 SUBPROGRAM 166. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.4 8–DIGIT PROGRAM NUMBER 170. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14. FUNCTIONS TO SIMPLIFY PROGRAMMING 173. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1 CANNED CYCLE 174. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.1 High–speed Peck Drilling Cycle (G73) 178. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.2 Left–handed Tapping Cycle (G74) 180. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.3 Fine Boring Cycle (G76) 182. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.4 Drilling Cycle, Spot Drilling (G81) 184. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.5 Drilling Cycle Counter Boring Cycle (G82) 186. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.6 Peck Drilling Cycle (G83) 188. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.7 Small–hole Peck Drilling Cycle (G83) 190. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.8 Tapping Cycle (G84) 194. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.9 Boring Cycle (G85) 196. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.10 Boring Cycle (G86) 198. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.11 Boring Cycle Back Boring Cycle (G87) 200. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.12 Boring Cycle (G88) 202. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.13 Boring Cycle (G89) 204. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.14 Canned Cycle Cancel (G80) 206. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2 RIGID TAPPING 209. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2.1 Rigid Tapping (G84) 210. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2.2 Left–handed Rigid Tapping Cycle (G74) 213. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2.3 Peck Rigid Tapping Cycle (G84 or G74) 216. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2.4 Canned Cycle Cancel (G80) 218. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3 CANNED GRINDING CYCLE (FOR GRINDING MACHINE) 219. . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.1 Plunge Grinding Cycle (G75) 220. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.2 Direct Constant–dimension Plunge Grinding Cycle (G77) 222. . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.3 Continuous–feed Surface Grinding Cycle (G78) 224. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.4 Intermittent–feed Surface Grinding Cycle (G79) 226. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–3

TABLE OF CONTENTS

14.4 GRINDING–WHEEL WEAR COMPENSATION BY CONTINUOUS DRESSING

(FOR GRINDING MACHINE) 228. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5 AUTOMATIC GRINDING WHEEL DIAMETER COMPENSATION AFTER DRESSING 229. . . . .

14.5.1 Checking the Minimum Grinding Wheel Diameter (for grinding machine) 229. . . . . . . . . . . . . . .

14.6 IN–FEED GRINDING ALONG THE Y AND Z AXES AT THE END OF TABLE SWING

(FOR GRINDING MACHINE) 230. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.7 OPTIONAL ANGLE CHAMFERING AND CORNER ROUNDING 231. . . . . . . . . . . . . . . . . . . . . . .

14.8 EXTERNAL MOTION FUNCTION (G81) 234. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.9 FIGURE COPY (G72.1, G72.2) 235. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.10 THREE–DIMENTIONAL COORDINATE CONVERSION (G68, G69) 242. . . . . . . . . . . . . . . . . . . . .

14.11 INDEX TABLE INDEXING FUNCTION 249. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–62764EN/01

15. COMPENSATION FUNCTION 252. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1 TOOL LENGTH OFFSET (G43,G44,G49) 253. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1.1 General 253. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1.2 G53, G28, G30, and G30.1 Commands in Tool Length Offset Mode 258. . . . . . . . . . . . . . . . . . . .

15.2 AUTOMATIC TOOL LENGTH MEASUREMENT (G37) 261. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3 TOOL OFFSET (G45–G48) 265. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.4 CUTTER COMPENSATION B (G39 – G42) 270. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.4.1 Cutter Compensation Left (G41) 273. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.4.2 Cutter Compensation Right (G42) 275. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.4.3 Corner Offset Circular Interpolation (G39) 277. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.4.4 Cutter Compensation Cancel (G40) 278. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.4.5 Switch between Cutter Compensation Left and Cutter Compensation Right 279. . . . . . . . . . . . . . .

15.4.6 Change of the Cutter Compensation Value 280. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.4.7 Positive/Negative Cutter Compensation Value and Tool Center Path 281. . . . . . . . . . . . . . . . . . . .

15.5 OVERVIEW OF CUTTER COMPENSATION C (G40 – G42) 283. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6 DETAILS OF CUTTER COMPENSA TION C 289. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.1 General 289. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.2 Tool Movement in Start–up 290. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.3 Tool Movement in Offset Mode 294. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.4 Tool Movement in Offset Mode Cancel 308. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.5 Interference Check 314. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.6 Overcutting by Cutter Compensation 319. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.7 Input Command from MDI 322. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.8 G53,G28,G30,G30.1 and G29 Commands in Cutter Compensation C Mode 323. . . . . . . . . . . . . .

15.7 THREE–DIMENSIONAL TOOL COMPENSATION (G40, G41) 342. . . . . . . . . . . . . . . . . . . . . . . . . .

15.8 TOOL COMPENSA–TION VALUES, NUMBER OF COMPENSATION VALUES,

AND ENTERING VALUES FROM THE PROGRAM (G10) 346. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.9 SCALING (G50,G51) 348. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.10 COORDINATE SYSTEM ROTATION (G68, G69) 353. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.11 NORMAL DIRECTION CONTROL (G40.1, G41.1, G42.1 OR G150, G151, G152) 359. . . . . . . . . . .

15.12 PROGRAMMABLE MIRROR IMAGE (G50.1, G51.1) 364. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.13 GRINDING WHEEL WEAR COMPENSATION 366. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16. CUSTOM MACRO 370. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.1 VARIABLES 371. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–4

B–62764EN/01

16.2 SYSTEM VARIABLES 375. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.3 ARITHMETIC AND LOGIC OPERATION 382. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.4 MACRO STATEMENTS AND NC STATEMENTS 386. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5 BRANCH AND REPETITION 387. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6 MACRO CALL 392. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.7 PROCESSING MACRO ST ATEMENTS 405. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.8 REGISTERING CUSTOM MACRO PROGRAMS 407. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.9 LIMITATIONS 408. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.10 EXTERNAL OUTPUT COMMANDS 409. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.11 INTERRUPTION TYPE CUSTOM MACRO 413. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

TABLE OF CONTENTS

16.5.1 Unconditional Branch (GOTO Statement) 387. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5.2 Conditional Branch (IF Statement) 388. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5.3 Repetition (While Statement) 389. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.1 Simple Call (G65) 393. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.2 Modal Call (G66) 397. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.3 Macro Call Using G Code 399. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.4 Macro Call Using an M Code 400. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.5 Subprogram Call Using an M Code 401. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.6 Subprogram Calls Using a T Code 402. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.7 Sample Program 403. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.11.1 Specification Method 414. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.11.2 Details of Functions 415. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

17. PATTERN DATA INPUT FUNCTION 423. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

17.1 DISPLAYING THE PATTERN MENU 424. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

17.2 PATTERN DATA DISPLAY 428. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

17.3 CHARACTERS AND CODES TO BE USED FOR THE PATTERN DATA INPUT FUNCTION 432.

18. PROGRAMMABLE PARAMETER ENTRY (G10) 434. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19. MEMORY OPERATION USING FS15 TAPE FORMAT 436. . . . . . . . . . . . . . . . . . . . . . . .

20. HIGH SPEED CUTTING FUNCTIONS 437. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.1 HIGH–SPEED CYCLE CUTTING 438. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.2 FEEDRATE CLAMPING BY ARC RADIUS 440. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.3 LOOK–AHEAD CONTROL (G08) 441. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.4 HIGH–SPEED REMOTE BUFFER 443. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.4.1 High–speed Remote Buffer A (G05) 443. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.4.2 High–speed Remote Buffer B (G05) 446. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.5 HIGH–PRECISION CONTOUR CONTROL 447. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.6 DISTRIBUTION PROCESSING TERMINATION MONITORING FUNCTION

FOR THE HIGH–SPEED MACHINING COMMAND (G05) 456. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21. AXIS CONTROL FUNCTIONS 457. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.1 SIMPLE SYNCHRONOUS CONTROL 458. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.2 ROTARY AXIS ROLL–OVER 461. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–5

TABLE OF CONTENTS

21.3 TOOL WITHDRAWAL AND RETURN (G10.6) 462. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.4 T ANDEM CONTROL 465. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.5 ANGULAR AXIS CONTROL/ANGULAR AXIS CONTROL B 466. . . . . . . . . . . . . . . . . . . . . . . . . .

21.6 CHOPPING FUNCTION (G80, G81.1) 468. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.7 SIMPLE ELECTRIC GEAR BOX (G80, G81) 474. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.8 RETREAT AND RETRY FUNCTIONS 479. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–62764EN/01

22. TWO–PATH CONTROL FUNCTION 485. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

22.1 GENERAL 486. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

22.2 WAITING FOR PATHS 487. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

22.3 MEMOR Y COMMON TO PATH 489. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

III. OPERATION

1. GENERAL 493. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.1 MANUAL OPERATION 494. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.2 TOOL MOVEMENT BY PROGRAMING– AUTOMATIC OPERATION 496. . . . . . . . . . . . . . . . . . . .

1.3 AUTOMATIC OPERATION 497. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4 TESTING A PROGRAM 499. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4.1 Check by Running the Machine 499. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4.2 How to View the Position Display Change without Running the Machine 500. . . . . . . . . . . . . . . .

1.5 EDITING A PART PROGRAM 501. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.6 DISPLAYING AND SETTING DATA 502. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7 DISPLAY 505. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.1 Program Display 505. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.2 Current Position Display 506. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.3 Alarm Display 506. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.4 Parts Count Display, Run Time Display 507. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.5 Graphic Display 507. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.8 DATA INPUT/OUTPUT 508. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2. OPERATIONAL DEVICES 509. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1 SETTING AND DISPLAY UNITS 510. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.1 9″ Monochrome CRT/MDI (Small Type) 511. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.2 9″ Monochrome CRT/MDI (Standard Type) 511. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.3 9″ Monochrome PDP/MDI (Standard Type) 512. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.4 8.4″ Color LCD/MDI (Small Type, Sheet Key) 512. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.5 8.4″ Color LCD/MDI (Standard Type, Sheet Key) 513. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.6 9.5″ Color LCD/MDI (Horizontal Type) 513. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.7 9.5″ Color LCD/MDI (Vertical Type) 514. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.8 14″ Color CRT/MDI (Horizontal Type) 515. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.9 14″ Color CRT/MDI (Vertical Type) 516. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.10 9″ Monochrome CRT (Separate Type) 517. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.11 9″ Monochrome PDP (Separate Type) 517. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.12 7.2″ Monochrome LCD (Separate type) 518. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–6

B–62764EN/01

2.2 EXPLANATION OF THE KEYBOARD 523. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3 FUNCTION KEYS AND SOFT KEYS 525. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4 EXTERNAL I/O DEVICES 546. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5 POWER ON/OFF 551. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

TABLE OF CONTENTS

2.1.13 8.4″ Color LCD (Separate type) 518. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.14 9.5″ Color LCD (Separate Type) 519. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.15 Separate Type MDI (Small Key) for 9″CRT/ PDP , 8.4″ /7.2 ″ LCD 519. . . . . . . . . . . . . . . . . . . . . . .

2.1.16 Separate Type MDI (Standard Key) for 9″CR T/PDP, 8.4″/7.2″LCD 520. . . . . . . . . . . . . . . . . . . . .

2.1.17 Separate Type MDI (Vertical Type) for 9.5″ LCD 521. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.18 Separate Type MDI (Horizontal Type) for 9.5 ″LCD 522. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.1 General Screen Operations 525. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.2 Function Keys 526. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.3 Soft Keys 527. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.4 Key Input and Input Buffer 543. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.5 Warning Messages 544. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.6 14″CRT and 9.5″LCD Soft Key Configuration 545. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.1 FANUC Handy File 548. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.2 FANUC Floppy Cassette 548. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.3 FANUC FA Card 549. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.4 FANUC PPR 549. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.5 Portable Tape Reader 550. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.1 Turning on the Power 551. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.2 Screen Displayed at Power–on 552. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.3 Power Disconnection 553. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3. MANUAL OPERATION 554. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.1 MANUAL REFERENCE POSITION RETURN 555. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.2 JOG FEED 557. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.3 INCREMENTAL FEED 559. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.4 MANUAL HANDLE FEED 560. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.5 MANUAL ABSOLUTE ON AND OFF 563. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.6 TOOL AXIS DIRECTION HANDLE FEED/TOOL AXIS DIRECTION HANDLE FEED B 568. . . . .

3.6.1 Tool Axis Direction Handle Feed 568. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.6.2 Tool Axis Normal Direction Handle Feed 571. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.7 MANUAL LINEAR/CIRCULAR INTERPOLATION 576. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.8 MANUAL RIGID TAPPING 581. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4. AUTOMATIC OPERATION 583. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.1 MEMOR Y OPERATION 584. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.2 MDI OPERATION 587. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.3 DNC OPERATION 591. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.4 SIMULTANEOUS INPUT/OUTPUT 594. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.5 PROGRAM REST ART 596. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.6 SCHEDULING FUNCTION 603. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.7 SUBPROGRAM CALL FUNCTION 608. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8 MANUAL HANDLE INTERRUPTION 610. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.9 MIRROR IMAGE 613. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–7

TABLE OF CONTENTS

4.10 TOOL WITHDRAWAL AND RETURN 615. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.11 RETRACE FUNCTION 621. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.12 MANUAL INTERVENTION AND RETURN 629. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.13 RETREAT AND RETRY FUNCTION 631. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–62764EN/01

5. TEST OPERATION 635. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.1 MACHINE LOCK AND AUXILIAR Y FUNCTION LOCK 636. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.2 FEEDRATE OVERRIDE 638. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.3 RAPID TRAVERSE OVERRIDE 639. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4 DRY RUN 640. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.5 SINGLE BLOCK 641. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6. SAFETY FUNCTIONS 643. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.1 EMERGENCY STOP 644. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.2 OVERTRAVEL 645. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.3 STROKE CHECK 646. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.4 STROKE LIMIT CHECK PRIOR TO PERFORMING MOVEMENT 650. . . . . . . . . . . . . . . . . . . . . . .

7. ALARM AND SELF–DIAGNOSIS FUNCTIONS 653. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1 ALARM DISPLAY 654. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2 ALARM HISTORY DISPLAY 656. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.3 CHECKING BY SELF–DIAGNOSTIC SCREEN 657. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8. DATA INPUT/OUTPUT 660. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1 FILES 661. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2 FILE SEARCH 663. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3 FILE DELETION 665. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4 PROGRAM INPUT/OUTPUT 666. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.1 Inputting a Program 666. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.2 Outputting a Program 668. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5 OFFSET DAT A INPUT AND OUTPUT 671. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5.1 Inputting Offset Data 671. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5.2 Outputting Offset Data 672. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6 INPUTTING AND OUTPUTTING PARAMETERS AND PITCH ERROR

COMPENSATION DATA 673. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.1 Inputting Parameters 673. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.2 Outputting Parameters 674. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.3 Inputting Pitch Error Compensation Data 675. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.4 Outputting Pitch Error Compensation Data 676. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.7 INPUTTING/OUTPUTTING CUSTOM MACRO COMMON VARIABLES 677. . . . . . . . . . . . . . . . .

8.7.1 Inputting Custom Macro Common Variables 677. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.7.2 Outputting Custom Macro Common Variable 678. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8 DISPLAYING DIRECTORY OF FLOPPY CASSETTE 679. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.1 Displaying the Directory 680. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.2 Reading Files 683. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.3 Outputting Programs 684. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.4 Deleting Files 685. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.9 OUTPUTTING A PROGRAM LIST FOR A SPECIFIED GROUP 687. . . . . . . . . . . . . . . . . . . . . . . . .

c–8

B–62764EN/01

TABLE OF CONTENTS

9. EDITING PROGRAMS 688. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1 INSERTING, ALTERING AND DELETING A WORD 689. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.1 Word Search 690. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.2 Heading a Program 692. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.3 Inserting a Word 693. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.4 Altering a Word 694. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.5 Deleting a Word 695. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2 DELETING BLOCKS 696. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.1 Deleting a Block 696. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.2 Deleting Multiple Blocks 697. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3 PROGRAM NUMBER SEARCH 698. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4 SEQUENCE NUMBER SEARCH 699. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5 DELETING PROGRAMS 701. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.1 Deleting One Program 701. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.2 Deleting All Programs 701. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.3 Deleting More Than One Program by Specifying a Range 702. . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6 EXTENDED PART PROGRAM EDITING FUNCTION 703. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.1 Copying an Entire Program 704. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.2 Copying Part of a Program 705. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.3 Moving Part of a Program 706. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.4 Mer ging a Program 707. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.5 Supplementary Explanation for Copying,Moving and Merging 708. . . . . . . . . . . . . . . . . . . . . . . .

9.6.6 Replacement of Words and Addresses 710. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.7 EDITING OF CUSTOM MACROS 712. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.8 BACKGROUND EDITING 713. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.9 PASSWORD FUNCTION 714. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10. CREATING PROGRAMS 716. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.1 CREATING PROGRAMS USING THE MDI PANEL 717. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2 AUTOMATIC INSERTION OF SEQUENCE NUMBERS 718. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.3 CREATING PROGRAMS IN TEACH IN MODE 720. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.4 CONVERSATIONAL PROGRAMMING WITH GRAPHIC FUNCTION 723. . . . . . . . . . . . . . . . . . . .

11. SETTING AND DISPLAYING DATA 727. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1 SCREENS DISPLAYED BY FUNCTION KEY 734. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.1 Position Display in the Work Coordinate System 735. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.2 Position Display in the Relative Coordinate System 737. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.3 Overall Position Display 740. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.4 Presetting the Workpiece Coordinate System 742. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.5 Actual Feedrate Display 743. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.6 Display of Run Time and Parts Count 745. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.7 Setting the Floating Reference Position 746. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.8 Operating Monitor Display 747. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2 SCREENS DISPLAYED BY FUNCTION KEY

(IN MEMORY MODE OR MDI MODE) 749. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

PROG

c–9

TABLE OF CONTENTS

11.2.1 Program Contents Display 750. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.2 Current Block Display Screen 751. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.3 Next Block Display Screen 752. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.4 Program Check Screen 753. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.5 Program Screen for MDI Operation 756. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.6 Stamping the Machining Time 757. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3 SCREENS DISPLAYED BY FUNCTION KEY

11.3.1 Displaying Memory Used and a List of Programs 765. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3.2 Displaying a Program List for a Specified Group 768. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4 SCREENS DISPLAYED BY FUNCTION KEY

11.4.1 Setting and Displaying the Tool Offset Value 772. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.2 Tool Length Measurement 775. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.3 Displaying and Entering Setting Data 777. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.4 Sequence Number Comparison and Stop 779. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.5 Displaying and Setting Run Time,Parts Count, and Time 781. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.6 Displaying and Setting the Workpiece Origin Offset Value 783. . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.7 Input of Measured Workpiece Origin Offsets 784. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.8 Displaying and Setting Custom Macro Common Variables 786. . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.9 Displaying Pattern Data and Pattern Menu 787. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.10 Displaying and Setting the Software Operator’s Panel 789. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.11 Displaying and Setting Tool Life Management Data 791. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.12 Displaying and Setting Extended T ool Life Management 794. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.13 Displaying and Setting Chopping Data 799. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

PROG

(IN THE EDIT MODE) 765. . . . . . . . . . . . . . .

OFFSET SETTING

B–62764EN/01

771. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5 SCREENS DISPLAYED BY FUNCTION KEY

SYSTEM

11.5.1 Displaying and Setting Parameters 802. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5.2 Displaying and Setting Pitch Error Compensation Data 804. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.6 DISPLAYING THE PROGRAM NUMBER, SEQUENCE NUMBER, AND STATUS,

AND WARNING MESSAGES FOR DATA SETTING OR INPUT/OUTPUT OPERATION 806. . . . .

11.6.1 Displaying the Program Number and Sequence Number 806. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.6.2 Displaying the Status and Warning for Data Setting or Input/Output Operation 807. . . . . . . . . . . .

11.7 SCREENS DISPLAYED BY FUNCTION KEY

MESSAGE

11.7.1 External Operator Message History Display 809. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8 CLEARING THE SCREEN 811. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8.1 Erase CRT Screen Display 811. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8.2 Automatic Erase CRT Screen Display 812. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12. GRAPHICS FUNCTION 813. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.1 GRAPHICS DISPLAY 814. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.2 DYNAMIC GRAPHIC DISPLAY 820. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.2.1 Path Drawing 820. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.2.2 Solid Graphics 829. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.3 BACKGROUND DRA WING 842. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

801. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

809. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13. HELP FUNCTION 845. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–10

B–62764EN/01

TABLE OF CONTENTS

IV. MAINTENANCE

1. METHOD OF REPLACING BATTERY 853. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.1 REPLACING CNC BATTERY FOR MEMORY BACK–UP 854. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.2 REPLACING BATTERIES FOR ABSOLUTE PULSE CODER 855. . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.3 REPLACING BATTERIES FOR ABSOLUTE PULSE CODER

( Series Servo Amp Module) 856. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

APPENDIX

A. TAPE CODE LIST 859. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B. LIST OF FUNCTIONS AND TAPE FORMAT 862. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

C. RANGE OF COMMAND VALUE 867. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D. NOMOGRAPHS 870. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D.1 INCORRECT THREADED LENGTH 871. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D.2 SIMPLE CALCULATION OF INCORRECT THREAD LENGTH 873. . . . . . . . . . . . . . . . . . . . . . . . .

D.3 TOOL PATH AT CORNER 875. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D.4 RADIUS DIRECTION ERROR AT CIRCLE CUTTING 878. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

E. STATUS WHEN TURNING POWER ON, WHEN CLEAR AND WHEN RESET 879. . . .

F. CHARACTER–TO–CODES CORRESPONDENCE TABLE 881. . . . . . . . . . . . . . . . . . . . . .

G. ALARM LIST 882. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

H. OPERATION OF PORTABLE TAPE READER 904. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–11

I. GENERAL

B–62764EN/01

GENERAL

This manual consists of the following parts:

1. GENERAL

  

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. When a program is created through conversational automatic programming function, refer to the manual for the conversational automatic programming function (Table 1).

III. OPERATION

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

IV. MAINTENANCE

Describes procedures for replacing batteries.

V. APPENDIX

Lists tape codes, valid data ranges, and error codes.

Some functions described in this manual may not be applied to some products. For detail, refer to the DESCRIPTIONS manual(B–62752EN).

This manual does not describe parameters in detail. For details on parameters mentioned in this manual, refer to the manual for parameters (B–62760EN).

This manual describes all optional functions. Look up the options incorporated into your system in the manual written by the machine tool builder.

The models covered by this manual, and their abbreviations are:

Product name Abbreviations

FANUC Series 16–MC 16–MC Series 16 FANUC Series 18–MC 18–MC Series 18 FANUC Series 160–MC 160–MC Series 160 FANUC Series 180–MC 180–MC Series 180

1. GENERAL

GENERAL

B–62764EN/01

Special symbols

Related manuals

This manual uses the following symbols:



Indicates a combination of axes such as

X__ Y__ Z (used in PROGRAMMING.).





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

The table below lists manuals related to MODEL C of Series 16, Series 18, Series 160 and Series 180. In the table, this manual is marked with an asterisk (*).

Table 1 Related Manuals

Manual name

DESCRIPTIONS B–62752EN CONNECTION MANUAL (Hardware) B–62753EN CONNECTION MANUAL (Function) B–62753EN–1 OPERATOR’S MANUAL for Lathe B–62754EN OPERATOR’S MANUAL for Machining Center B–62764EN

Specification

number

MAINTENANCE MANUAL B–62755 PARAMETER MANUAL B–62760EN PROGRAMMING MANUAL (Macro Compiler / Macro Executer) B–61803E–1 FAPT MACRO COMPILER PROGRAMMING MANUAL B–66102E FANUC Super CAP T/Super CAP II T OPERATOR’S MANUAL B–62444E–1 FANUC Super CAP M/Super CAP II M OPERATOR’S MANUAL B–62154E FANUC Super CAP M PROGRAMMING MANUAL B–62153E CONVERSATIONAL AUTOMATIC PROGRAMMING FUNCTION I

for Lathe OPERATOR’S MANUAL CONVERSATIONAL AUTOMATIC PROGRAMMING FUNCTION II

for Lathe OPERATOR’S MANUAL CONVERSATIONAL AUTOMATIC PROGRAMMING FUNCTION

for MACHINING CENTER OPERATOR’S MANUAL

B–61804E–1

B–61804E–2

B–61874E–1

B–62764EN/01

Machining rocess

GENERAL

1. GENERAL

1.1

GENERAL FLOW OF OPERATION OF CNC MACHINE TOOL

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

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

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

Part drawing

CHAPTER II PROGRAMMING CHAPTER III OPERATION

Part programming

CNC

MACHINE TOOL

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

1. Determination of workpieces machining range

2. Method of mounting workpieces on the machine tool

3. Machining sequence in every machining process

4. Machining tools and machining

Decide the machining method in every machining process.

Machining process

Machining procedure

1. Machining method : Rough Semi Finish

2. Machining tools

3. Machining conditions : Feedrate Cutting depth

4. Tool path

1 2 3

Feed cutting Side cutting

Hole

machining

1. GENERAL

GENERAL

Tool

Side cutting

B–62764EN/01

Face cutting

Hole machining

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

B–62764EN/01

1.2

NOTES ON READING THIS MANUAL

GENERAL

NOTE

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 Headings are placed in the left margin so that the reader can

easily access necessary information. When locating the necessary information, the reader can save time by searching though these headings.

3 Machining programs, parameters, variables, 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.

4 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. GENERAL

II. PROGRAMMING

B–62764EN/01



PROGRAMMING

1. GENERAL

PROGRAMMING

B–62764EN/01

1.1 TOOL MOVEMENT ALONG WORKPIECE PARTS FIGURE– INTERPOLATION

Explanations

D Tool movement along a

straight line

The tool moves along straight lines and arcs constituting the workpiece parts figure (See II–4).

The function of moving the tool along straight lines and arcs is called the interpolation.

Tool

Workpiece

Fig.1.1 (a) Tool movement along a straight line

Program G01 X_ _ Y_ _ ; X_ _ ;

D Tool movement along an

arc

Program G03X_ _Y_ _R_ _;

Tool

Workpiece

Fig. 1.1 (b) T ool movement along an arc

B–62764EN/01

PROGRAMMING

1. GENERAL

Symbols of the programmed commands G01, G02, ... are called the preparatory function and specify the type of interpolation conducted in the control unit.

(a) Movement along straight line

G01 Y_ _; X– –Y– – – –;

Control unit

Interpolation

a)Movement

along straight line

b)Movement

along arc

Fig. 1.1 (c) Interpolation function

(b) Movement along arc

G03X––Y––R––;

X axis

Y axis

Tool movement

NOTE

Some machines move tables instead of tools but this manual assumes that tools are moved against workpieces.

1. GENERAL

PROGRAMMING

B–62764EN/01

1.2

FEED– FEED FUNCTION

Movement of the tool at a specified speed for cutting a workpiece is called the feed.

mm/min

Workpiece

Table

Fig. 1.2 (a) Feed function

Tool

Feedrates can be specified by using actual numerics. For example, to feed the tool at a rate of 150 mm/min, specify the following in the program: F150.0 The function of deciding the feed rate is called the feed function (See II–5).

B–62764EN/01

1.3 PART DRAWING AND TOOL MOVEMENT

PROGRAMMING

1. GENERAL

1.3.1

Reference Position (Machine–Specific Position)



A CNC machine tool is provided with a fixed position. Normally, tool change and programming of absolute zero point as described later are performed at this position. This position is called the reference position.

Reference position

Tool

Workpiece

Table

Fig. 1.3 (a) Reference position

The tool can be moved to the reference position in two ways: (1)Manual reference position return (See III–3.1)

Reference position return is performed by manual button operation.

(2)Automatic reference position return (See II–6)

In general, manual reference position return is performed first after the power is turned on. In order to move the tool to the reference position for tool change thereafter, the function of automatic reference position return is used.

1. GENERAL

1.3.2

Coordinate System on Part Drawing and Coordinate System Specified by CNC – Coordinate System

PROGRAMMING

B–62764EN/01

Program

Explanations

D Coordinate system

Part drawing

Fig. 1.3.2 (a)

Coordinate system

CNC

Command

Tool

Workpiece

Machine tool

Coordinate system

The following two coordinate systems are specified at different locations: (See II–8)

(1)Coordinate system on part drawing

The coordinate system is written on the part drawing. As the program data, the coordinate values on this coordinate system are used.

(2)Coordinate system specified by the CNC

The coordinate system is prepared on the actual machine tool table. This can be achieved by programming the distance from the current position of the tool to the zero point of the coordinate system to be set.

230

300

Program zero point

Fig. 1.3.2 (b) Coordinate system specified by the CNC

Present tool position

Distance to the zero point of a coordinate system to be set

B–62764EN/01

PROGRAMMING

1. GENERAL

The positional relation between these two coordinate systems is determined when a workpiece is set on the table.

Coordinate system on part drawing established on the work-

Coordinate system specified by the CNC established on the table

Table

Fig. 1.3.2 (c) Coordinate system specified by CNC and coordinate

systemon part drawing

Workpiece

piece

D Methods of setting the

two coordinate systems in the same position

The tool moves on the coordinate system specified by the CNC in accordance with the command program generated with respect to the coordinate system on the part drawing, and cuts a workpiece into a shape on the drawing. Therefore, in order to correctly cut the workpiece as specified on the drawing, the two coordinate systems must be set at the same position.

To set the two coordinate systems at the same position, simple methods shall be used according to workpiece shape, the number of machinings.

(1)Using a standard plane and point of the workpiece.

Fixed distance

Program zero point

Bring the tool center to the workpiece standard point. And set the coordinate system specified by CNC at this position.

Workpiece’s standard point

Fixed distance

1. GENERAL

PROGRAMMING

B–62764EN/01

(2)Mounting a workpiece directly against the jig

Program zero point

Jig

Meet the tool center to the reference position. And set the coordinate system specified by CNC at this position. (Jig shall be mounted on the predetermined point from the reference position.)

(3)Mounting a workpiece on a pallet, then mounting the workpiece and

pallet on the jig

Pallet

Jig

Workpiece

(Jig and coordinate system shall be specified by the same as (2)).

B–62764EN/01

1.3.3

How to Indicate Command Dimensions for Moving the Tool – Absolute, Incremental Commands

PROGRAMMING

1. GENERAL

Explanations

D Absolute command

Command for moving the tool can be indicated by absolute command or incremental command (See II–9.1).

The tool moves to a point at “the distance from zero point of the coordinate system” that is to the position of the coordinate values.

Command specifying movement from point A to point B



B(10.0,30.0,20.0)

G90 X10.0 Y30.0 Z20.0 ;

Coordinates of point B

Tool

D Incremental command

Specify the distance from the previous tool position to the next tool position.

Tool

X=40.0



Z=–10.0

Command specifying movement from point A to point B

Y=–30.0

G91 X40.0 Y–30.0 Z–10.0

Distance and direction for movement along each axis

;

1. GENERAL

PROGRAMMING

B–62764EN/01

1.4

CUTTING SPEED – SPINDLE SPEED FUNCTION

Examples

The speed of the tool with respect to the workpiece when the workpiece is cut is called the cutting speed. As for the CNC, the cutting speed can be specified by the spindle speed in rpm unit.

Tool

Spindle speed N

rpm

Workpiece

Tool diameter  D mm

V: Cutting speed

m/min

The spindle speed is approximately 250 rpm, which is obtained from N=1000v/πD. Hence the following command is required:

S250; Commands related to the spindle speed are called the spindle speed function ( See II–10) .

B–62764EN/01

PROGRAMMING

1. GENERAL

1.5

SELECTION OF TOOL USED FOR VARIOUS MACHINING – TOOL FUNCTION

Examples

When drilling, tapping, boring, milling or the like, is performed, it is necessary to select a suitable tool. When a number is assigned to each tool and the number is specified in the program, the corresponding tool is selected.

Tool number

01 02

A TC magazine

When the tool is stored at location 01 in the ATC magazine, the tool can be selected by specifying T01. This is called the tool function (See II–11).

1. GENERAL

PROGRAMMING

B–62764EN/01

1.6

COMMAND FOR MACHINE OPERATIONS – MISCELLANEOUS FUNCTION

When machining is actually started, it is necessary to rotate the spindle, and feed coolant. For this purpose, on–off operations of spindle motor and coolant valve should be controlled.

Tool

Coolant

Workpiece

The function of specifying the on–off operations of the components of the machine is called the miscellaneous function. In general, the function is specified by an M code (See II–12). For example, when M03 is specified, the spindle is rotated clockwise at the specified spindle speed.

B–62764EN/01

PROGRAMMING

1. GENERAL

1.7

PROGRAM CONFIGURATION

A group of commands given to the CNC for operating the machine is called the program. By specifying the commands, the tool is moved along a straight line or an arc, or the spindle motor is turned on and off. In the program, specify the commands in the sequence of actual tool movements.

Block

Tool movement sequence

Block

Program

Fig. 1.7 (a) Program configuration

Block

⋅ ⋅ ⋅ ⋅

Block

A group of commands at each step of the sequence is called the block. The program consists of a group of blocks for a series of machining. The number for discriminating each block is called the sequence number, and the number for discriminating each program is called the program number (See II–13).

1. GENERAL

PROGRAMMING

B–62764EN/01

Explanations

D Block

D Program

The block and the program have the following configurations.

1 block

N ffff G ff Xff.f Yfff.f M ff S ff T ff ;

Sequence number

Preparatory function

Dimension word Miscel-

laneous function

Fig. 1.7 (b) Block configuration

Spindle function

Tool function

End of block

A block starts with a sequence number to identify the block and ends with an end–of–block code. This manual indicates the end–of–block code by ; (LF in the ISO code and CR in the EIA code).

;

Offff;

⋅ ⋅ ⋅

M30 ;

Fig. 1.7 (c) Program configuration

Program number

Bloc k Bloc k

⋅

Bloc

⋅

End of program

Normally , a program number is specified after the end–of–block (;) code at the beginning of the program, and a program end code (M02 or M30) is specified at the end of the program.

B–62764EN/01

PROGRAMMING

1. GENERAL

D Main program and

subprogram

When machining of the same pattern appears at many portions of a program, a program for the pattern is created. This is called the subprogram. On the other hand, the original program is called the main program. When a subprogram execution command appears during execution of the main program, commands of the subprogram are executed. When execution of the subprogram is finished, the sequence returns to the main program.

Main program

⋅ ⋅

M98P1001

⋅ ⋅ ⋅

M98P1002

⋅ ⋅ ⋅

M98P1001

⋅ ⋅

Subprogram #1

O1001

M99

Subprogram #2

O1002

Program for hole #1

Program for hole #2

⋅

M99

Hole #1

Hole #2

1. GENERAL

1.8

TOOL FIGURE AND TOOL MOTION BY PROGRAM

Explanations

PROGRAMMING

B–62764EN/01

D Machining using the end

of cutter – Tool length compensation function (See II–15.1)

D Machining using the side

of cutter – Cutter compensation function (See II–15.4,15.5,15.6)

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 (data display and setting : see III–11), machining can be performed without altering the program even when the tool is changed. This function is called tool length compensation.

Standard tool

Workpiece

H3 H4

Because a cutter has a radius, the center of the cutter path goes around the workpiece with the cutter radius deviated.

Cutter path using cutter compensation

Machined part figure

Workpiece

Cutter

If radius of cutters are stored in the CNC (Data Display and Setting : see III–11), the tool can be moved by cutter radius apart from the machining part figure. This function is called cutter compensation.

B–62764EN/01

PROGRAMMING

1. GENERAL

1.9

TOOL MOVEMENT RANGE – STROKE

Limit switches are installed at the ends of each axis on the machine to prevent tools from moving beyond the ends. The range in which tools can move is called the stroke.

Table

Motor

Limit switch

Machine zero point

Specify these distances.

Tools cannot enter this area. The area is specified by data in memory or a program.

Besides strokes defined with limit switches, the operator can define an area which the tool cannot enter using a program or data in memory . This function is called stroke check (see III–6.3).

2. CONTROLLED AXES

CONTROLLED AXES

PROGRAMMING

B–62764EN/01

2.1 CONTROLLED AXES

PROGRAMMING

2. CONTROLLED AXES

Series 16, Series 160

Series 18, Series 180

Item

No. of basic controlled axes

Controlled axes expansion (total)

Basic simultaneously controlled axes

Simultaneously controlled axes expansion (total)

16–MC

160–MC

3 axes Max. 8 axes

(included in Cs axis) 2 axes

Max. 6 axes Max. 6 axes for each path

16–MC, 160–MC

(two–path control)

3 axes for each path (6 axes in total)

Max. 7 axes for each path (Feed 6 axes + Cs axis)

2 axes for each path (4 axes in total)

NOTE

The number of simultaneously controllable axes for manual operation jog feed, manual reference position return, or manual rapid traverse) is 1 or 3 (1 when bit 0 (JAX) of parameter 1002 is set to 0 and 3 when it is set to 1).

Item 18–MC, 180–MC

No. of basic controlled axes 3 axes Controlled axes expansion (total) Basic simultaneously controlled axes 2 axes

Simultaneously controlled axes expansion (total) Max. 4 axes

Max. 6 axes (included in Cs axis)

2.2 AXIS NAME

NOTE

The user can assign any one of the following nine characters as the axis name: A, B, C, U, V, W, X, Y, and Z.Parameter No. 1020 is used to determine the name of each axis. When this parameter is set to 0 or a character other than the valid characters is specified, an axis name from 1 to 8 is assigned by default. In two–path control, the basic three axis names are fixed to X, Y, and Z for either path, but the name of an additional axis can be selected from A, B, C, U, V, and W by parameter 1020. Duplicate axis names cannot be used in the same path, but the same axis name can be used in different paths.

2. CONTROLLED AXES

Limitations

PROGRAMMING

B–62764EN/01

D Default axis name

D Duplicate axis names

When a default axis name (1 to 8) is used, operation in the MEM mode and MDI mode is disabled.

If a duplicate axis name is specified in the parameter, operation is enabled only for the axis specified first.

NOTE

In two–path control, axis information displayed on the CRT screen, such as the current position, may contain an axis name with a suffix indicating the related path (X1, X2, etc). This is intended to provide a comprehensible indication of the path to which the axis belongs. The suffix cannot be used in a program ; the axis name should be specified as X, Y, Z, U, V, W, A, B, or C.

B–62764EN/01

PROGRAMMING

2. CONTROLLED AXES

2.3 INCREMENT SYSTEM

The increment system consists of the least input increment (for input) and least command increment (for output). The least input increment is the least increment for programming the travel distance. The least command increment is the least increment for moving the tool on the machine. Both increments are represented in mm, inches, or deg.

Name of increment system

IS–B

Name of increment system

IS–C

Least input increment

0.001mm

0.0001inch

0.001deg Least input incre-

ment

0.0001mm

0.00001inch

0.0001deg

Least command increment

0.001mm

0.0001inch

0.001deg Least command

increment

0.0001mm

0.00001inch

0.0001deg

Maximum stroke

99999.999mm

9999.9999inch

99999.999deg Maximum

stroke

9999.9999mm

999.99999inch

9999.9999deg

The least command increment is either metric or inch depending on the machine tool. Set metric or inch to the parameter INM (No.100#0). For selection between metric and inch for the least input increment, G code (G20 or G21) or a setting parameter selects it.

Combined use of the inch system and the metric system is not allowed. There are functions that cannot be used between axes with different unit systems (circular interpolation, cutter compensation, etc.). For the increment system, see the machine tool builder’s manual.

2. CONTROLLED AXES

IS–B

IS–C

PROGRAMMING

B–62764EN/01

2.4 MAXIMUM STROKE

Maximum stroke = Least command increment  99999999 See 2.3 Incremen System.

Table 2.4(a) Maximum strokes

Increment system Maximum stroke

Metric machine system 99999.999 mm

99999.999 deg

–

Inch machine system 9999.9999 inch

99999.999 deg

Metric machine system 9999.9999 mm

9999.9999 deg

–

Inch machine system 999.99999 inch

9999.9999 deg

NOTE

1 A command exceeding the maximum stroke cannot be

specified.

2 The actual stroke depends on the machine tool.

B–62764EN/01

3. PREP ARATORY FUNCTION

PROGRAMMING

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.

(G FUNCTION)

G01X 

Z X

G00Z

G01 is effective in this range.



3. PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING

B–62764EN/01

Explanations

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

indicated in Table 3.

(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 parameter G23 (No.

3402#7). 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.

(6) The user can select G17, G18, or G19 by setting bit 1 (parameterG18)

and bit 2 (parameter G19) of parameter No. 3402.

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, P/S alarm No. 010 is output.

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 canned cycle, the canned cycle 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.G codes are indicated by group.

B–62764EN/01

3. PREP ARATORY FUNCTION

PROGRAMMING

Table 3 G code list (1/3)

G code

G00 G01 G02 G03 G02.2, G03.2 G02.3, G03.3 G04 Dwell, Exact stop G05 High speed cycle machining G07.1 (G107) Cylindrical interpolation G08 G09 G10 Programmable data input G10.6 Tool retract & recover G11 Programmable data input mode cancel G12.1

G13.1 G15 G16 G17

G18

G19 G20 G21

G22 G23 G25

G26 G27 Reference position return check G28 Return to reference position G29 G30 G30.1 Floating reference point return G31 Skip function G33 01 Thread cutting

Group Function

Positioning Linear interpolation

02 ZpXp plane selection Yp: Y axis or its parallel axis

Circular interpolation/Helical interpolation CW Circular interpolation/Helical interpolation CCW Involute interpolation Explanation interpolation

Look–ahead control Exact stop

Polar coordinate interpolation mode Polar coordinate interpolation cancel mode Polar coordinates command cancel Polar coordinates command XpY p plane selection Xp: X axis or its parallel axis

Y pZp plane selection Zp: Z axis or its parallel axis Input in inch Input in mm Stored stroke check function on Stored stroke check function off Spindle speed fluctuation detection off Spindle speed fluctuation detection on

Return from reference position 2nd, 3rd and 4th reference position return

(G FUNCTION)

3. PREPARATORY FUNCTION

(G FUNCTION)

G code

G37 G39 G40 G41 G42 Cutter compensation right G40.1 (G150)

G41.1 (G151) 19 Normal direction control left side on G42.1 (G152) Normal direction control right side on G43 G44 G45 Tool offset increase G46

G47 G48 Tool offset double decrease G49 G50 G51 G50.1

G51.1 G52 G53 G54 G54.1 Additional workpiece coordinate system selection

G55 G56 G57 Workpiece coordinate system 4 selection G58 Workpiece coordinate system 5 selection G59 Workpiece coordinate system 6 selection G60 00 Single direction positioning G61 Exact stop mode G62 G63 G64

PROGRAMMING

Table 3 G code list (2/3)

Group Function

Automatic tool length measurment Corner offset circular interpolation Cutter compensation cancel/Three dimensional compensation cancel

08 Tool length compensation cancel

Cutter compensation left/Three dimensional compensation

Normal direction control cancel mode

Tool length compensation + direction Tool length compensation – direction

Tool offset decrease Tool offset double increase

Scaling cancel Scaling Programmable mirror image cancel Programmable mirror image Local coordinate system setting Machine coordinate system selection Workpiece coordinate system 1 selection

Workpiece coordinate system 2 selection Workpiece coordinate system 3 selection

Automatic corner override Tapping mode Cutting mode

B–62764EN/01

3. PREP ARATORY FUNCTION

PROGRAMMING

Table 3 G code list (3/3)

G code

G65 00 Macro call G66

G67 G68

G69 G73 G74 G75 01 Plunge grinding cycle (for grinding machine)

G76 G77 Direct constant–dimension plunge grinding cycle(for grinding machine) G78 01 Continuous–feed surface grinding cycle(for grinding machine) G79 Intermittent–feed surface grinding cycle(for grinding machine)

G80 G81

G82 Drilling cycle or counter boring cycle G83 Peck drilling cycle G84 G85 Boring cycle G86 Boring cycle G87 Back boring cycle G88 Boring cycle G89 Boring cycle G90 G91 G92 G92.1 G94 G95 G96 G97 G98 G99 G160 G161

Group Function

Macro modal call Macro modal call cancel Coordinate rotation Coordinate rotation cancel Peck drilling cycle Counter tapping cycle

Fine boring cycle

Canned cycle cancel/external operation function cancel Drilling cycle, spot boring cycle or external operation function

Tapping cycle

Absolute command Increment command Setting for work coordinate system or clamp at maximum spindle speed Workpiece coordinate system preset Feed per minute Feed per rotation Constant surface speed control Constant surface speed control cancel Return to initial point in canned cycle Return to R point in canned cycle In–feed control function cancel(for grinding machine) In–feed control function(for grinding machine)

(G FUNCTION)

4. INTERPOLA TION FUNCTIONS

INTERPOLATION FUNCTIONS

PROGRAMMING

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.1

POSITIONING (G00)

Format

Explanations

The G00 command moves a tool to the position in the workpiece system specified with an absolute or an incremental command at a rapid traverse rate. In the absolute command, coordinate value of the end point is programmed. In the incremental command the distance the tool moves is programmed.

G00IP_;

IP_: For an absolute command, the coordinates of an end

position, and for an incremental commnad, the distance the tool moves.

Either of the following tool paths can be selected according to bit 1 of parameter LRP No. 1401.

D Nonlinear interpolation positioning

The tool is positioned with the rapid traverse rate for each axis separately. The tool path is normally straight.

D Linear interpolation positioning

The tool path is the same as in linear interpolation (G01). The tool is positioned within the shortest possible time at a speed that is not more than the rapid traverse rate for each axis.

Start position

Linear interpolation positioning

End position

Non linear interpolation positioning

The rapid traverse rate in G00 command is set to the parameter No. 1420 for each axis independently by the machine tool builder. In the posiitoning mode actuated by G00, the tool is accelerated to a predetermined speed at the start of a block and is decelerated at the end of a block. Execution proceeds to the next block after confirming the in–position. “In–position ” means that the feed motor is within the specified range. This range is determined by the machine tool builder by setting to parameter (No. 1826). In–position check for each block can be disabled by setting bit 5 (NCI) of parameter No.1601 accordingly.

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62764EN/01

Limitations

The rapid traverse rate cannot be specified in the address F. Even if linear interpolation positioning is specified, nonlinear interpolation positioning is used in the following cases. Therefore, be careful to ensure that the tool does not foul the workpiece. D G28 specifying positioning between the reference and intermediate

positions.

D G53

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.2

SINGLE DIRECTION POSITIONING (G60)

Format

For accurate positioning without play of the machine (backlash), final positioning from one direction is available.

Overrun

Start position

End position

G60 IP_;

IP_ : For an absolute command, the coordinates of an end

position, and for an incremental commnad, the distance the tool moves.

Temporary stop

Explanations

Examples

An overrun and a positioning direction are set by the parameter (No.

5440). Even when a commanded positioning direction coincides with that set by the parameter, the tool stops once before the end point. G60, which is an one–shot G–code, can be used as a modal G–code in group 01 by setting 1 to the parameter (No. 5431 bit 0 MDL). This setting can eliminate specifying a G60 command for every block. Other specifications are the same as those for an one–shot G60 command. When an one–shot G code is sepcified in the single direction positioning mode, the one–shot G command is effective like G codes in group 01.

When one–shot G60 commands are used.

G90; G60 X0Y0; G60 X100; G60 Y100; G04 X10; G00 X0Y0;

Single direction positioning

When modal G60 command is used.

G90G60; X0Y0; X100; Y100; G04X10; G00X0Y0;

Single direction positioning mode start

Single direction positioning

Dwell Single direction

positioning mode cancel

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62764EN/01

Restrictions

D During canned cycle for drilling, no single direction positioning is

effected in Z axis.

D No single direction positioning is effected in an axis for which no

overrun has been set by the parameter.

D When the move distance 0 is commanded, the single direction

positioning is not performed.

D The direction set to the parameter is not effected by mirror image. D The single direction positioning does not apply to the shift motion in

the canned cycles of G76 and G87.

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.3

LINEAR INTERPOLATION (G01)

Format

Explanations

Tools can move along a line

G01 IP_F_;

IP_:For an absolute command, the coordinates of an end point ,

and for an incremental commnad, the distance the tool moves.

F_:Speed of tool feed (Feedrate)

A tools move along a line to the specified position at the feedrate specified in F. The feedrate specified in F is effective until a new value is specified. It need not be specified for each block. The feedrate commanded by the F code is measured along the tool path. If the F code is not commanded, the feedrate is regarded as zero. The feedrate of each axis direction is as follows.

G01ααββγγζζ

Feed rate of α axis direction :

Feed rate of Β axis direction :

Feed rate of Γ axis direction :

Feed rate of Ζ axis direction :

L + a

) b2) g2) z

Ff ;

Fa +

Fb+

Fg +

The feed rate of the rotary axis is commanded in the unit of deg/min (the unit is decimal point position).

When the straight line axis α(such as X, Y, or Z) and the rotating axisβ (such as A, B, or C) are linearly interpolated, the feed rate is that in which the tangential feed rate in the αandβ cartesian coordinate system is commanded by F(mm/min). β–axis feedrate is obtained ; at first, the time required for distribution is calculated by using the above fromula, then the β –axis feedrate unit is changed to deg 1min.

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62764EN/01

A calcula;tion example is as follows. G91 G01 X20.0B40.0 F300.0 ; This changes the unit of the C axis from 40.0 deg to 40mm with metric input. The time required for distribution is calculated as follows:

Examples

D Linear interpolation

202) 40

The feed rate for the C axis is

300

0.14907

0.14907 (min)8

268.3 degńmin

In simultaneous 3 or 4 axes control, the feed rate is calculated the same way as in 2 axes control.

(G91) G01X200.0Y100.0F200.0 ;

Y axis

100.0

(End position)

D Feedrate for the

rotation axis

(Start position)

G91G01C–90.0 G300.0 ;Feed rate of 300deg/min

(End point)

200.00

(Start point)

90°

Feedrate is 300 deg/min

X axis

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.4

CIRCULAR INTERPOLATION (G02,G03)

Format

The command below will move a tool along a circular arc.

Arc in the XpYp plane

G17

Arc in the ZpXp plane

G18

Arc in the YpZp plane

G19

G02 G03

Xp_Yp_

Xp_ p_

Yp_ Zp_

I_ J_ R_

I_ K_ R_

J_ K_

F_ ;

T able.4.4 Description of the Command Format

Command

G17 Specification of arc on XpYp plane G18 Specification of arc on ZpXp plane G19 Specification of arc on YpZp plane G02 Circular Interpolation Clockwise direction (CW) G03 Circular Interpolation Counterclockwise direction (CCW)

I_ Xp axis distance from the start point to the center of an arc

J_ Yp axis distance from the start point to the center of an arc

Command values of X axis or its parallel axis (set by parameter No. 1022)

Command values of Y axis or its parallel axis (set by parameter No. 1022)

Command values of Z axis or its parallel axis (set by parameter No. 1022)

with sign

Description

k_ Zp axis distance from the start point to the center of an arc

with sign R_ Arc radius (with sign) F_ Feedrate along the arc

4. INTERPOLA TION FUNCTIONS

Explanations

PROGRAMMING

B–62764EN/01

D Direction of the circular

interpolation

D Distance moved on an

arc

D Distance from the start

point to the center of arc

“Clockwise”(G02) and “counterclockwise”(G03) on the XpYp plane (Z

plane or YpZp plane) are defined when the XpYp plane is viewed

pXp

in the positive–to–negative direction of the Z

axis (Yp axis or Xp axis,

respectively) in the Cartesian coordinate system. See the figure below.

Yp Xp Zp

G18

G03

G02

G19

G02

G17

G03

G02

The end point of an arc is specified by address Xp, Yp or Zp, and is expressed as an absolute or incremental value according to G90 or G91. For the incremental value, the distance of the end point which is viewed from the start point of the arc is specified.

The arc center is specified by addresses I, J, and K for the Xp, Y p, and Zp axes, respectively . The numerical value following I, J, or K, however, is a vector component in which the arc center is seen from the start point, and is always specified as an incremental value irrespective of G90 and G91, as shown below. I, J, and K must be signed according to the direction.

End point (x,y)

Center

Start point

I0,J0, and K0 can be omitted. When Xp, Yp , and Z

End point (z,x)

Center

Start point

End point (y ,z)

Center

are omitted (the end

Start point

point is the same as the start point) and the center is specified with I, J, and K, a 360° arc (circle) is specified. G021; Command for a circle If the difference between the radius at the start point and that at the end point exceeds the permitted value in a parameter (No.3410), an P/S alarm (No.020) occurs.

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

D  

The distance between an arc and the center of a circle that contains the arc can be specified using the radius, R, of the circle instead of I, J, and K. In this case, one arc is less than 180°, and the other is more than 180° are considered. When an arc exceeding 180° is commanded, the radius must be specified with a negative value. If Xp, Yp, and Zp are all omitted, if the end point is located at the same position as the start point and when R is used, an arc of 0° is programmed G02R ; (The cutter does not move.)

For arc (1)(less than 180°)

G91 G02 X

For arc (2)(greater than 180°)

G91 G02 X

60.0 YP20.0 R50.0 F300.0 ;

60.0 YP20.0 R–50.0 F300.0 ;

r=50mm

End point

D 

Restrictions

Start point

r=50mm

The feedrate in circular interpolation is equal to the feed rate specified by the F code, and the feedrate along the arc (the tangential feedrate of the arc) is controlled to be the specified feedrate. The error between the specified feedrate and the actual tool feedrate is ±2% or less. However, this feed rate is measured along the arc after the cutter compensation is applied

If I, J, K, and R addresses are specified simultaneously, the arc specified by address R takes precedence and the other are ignored. If an axis not comprising the specified plane is commanded, an alarm is displayed. For example, if axis U is specified as a parallel axis to X axis when plane XY is specified, an P/S alarm (No.028)is displayed. When an arc having a center angle approaching 180° is specified, the calculated center coordinates may contain an error. In such a case, specify the center of the arc with I, J, and K.

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62764EN/01

Examples

Y axis

100

50R

140

60R

200

60 40

90 120

The above tool path can be programmed as follows ;

   

G92X200.0 Y40.0 Z0 ; G90 G03 X140.0 Y100.0R60.0 F300.; G02 X120.0 Y60.0R50.0 ;

G92X200.0 Y40.0Z0 ; G90 G03 X140.0 Y100.0I-60.0 F300.; G02 X120.0 Y60.0I-50.0 ;

   

G91 G03 X-60.0 Y60.0 R60.0 F300.; G02 X-20.0 Y-40.0 R50.0 ;

G91 G03 X-60.0 Y60.0 I-60.0 F300. ; G02 X-20.0 Y-40.0 I-50.0 ;

X axis

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.5

HELICAL INTERPOLATION (G02,G03)

Format

Helical interpolation which moved helically is enabled by specifying up to two other axes which move synchronously with the circular interpolation by circular commands.

Synchronously with arc of XpYp plane

G17

Synchronously with arc of ZpXp plane

G18

Synchronously with arc of YpZp plane

G19

α,β:Any one axis where circular interpolation is not applied

G02 G03

Up to two other axes can be specified.

XpYp

XpZp

YpZp

IJ R_

IK



JK R

α(β)F

αβ)F_;

αβ)F;

Explanations

The command method is to simply or secondary add a move command axis which is not circular interpolation axes. An F command specifies a feed rate along a circular arc. Therefore, the feed rate of the linear axis is as follows:

Length of linear axis

F×

Length of circular arc

Determine the feed rate so the linear axis feed rate does not exceed any of the various limit values.Bit 0 (HFC) of parameter No. 1404 can be used to prevent the linear axis feedrate from exceeding various limit values.

Tool path

Restrictions

The feedrate along the circumference of two circular interpolated axes is the specified feedrate.

⋅Cutter compensation is applied only for a circular arc. ⋅Tool offset and tool length compensation cannot be used in a block in

which a helical interpolation is commanded.

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62764EN/01

4.6

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

Format

D Specify G12.1 and G13.1

in Separate Blocks.

Explanations

D Polar coordinate

interpolation plane

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

G12.1 ;

G13.1 ;

Starts polar coordinate interpolation mode (enables polar

coordinate interpolation)

Specify linear or circular interpolation using coordinates in a

Cartesian coordinate system consisting of a linear axis and

rotary axis (virtual axis).

Polar coordinate interpolation mode is cancelled (for not

performing polar coordinate interpolation)

G12.1 starts the polar coordinate interpolation mode and selects a polar coordinate interpolation plane (Fig. 4.6 (a)). Polar coordinate interpolation is performed on this plane.

Rotary axis (virtual axis) (unitmm or inch)

Linear axis (unit:mm or inch)

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

Fig4.6 (a) Polar coordinate interpolation plane.

When the power is turned on or the system is reset, polar coordinate interpolation is canceled (G13.1). The linear and rotation axes for polar coordinate interpolation must be set in parameters (No. 5460 and 5461) beforehand.

CAUTION

The plane used before G12.1 is specified (plane selected by G17, G18, or G19) is canceled. It is restored when G13.1 (canceling polar coordinate interpolation) is specified. When the system is reset, polar coordinate interpolation is canceled and the plane specified by G17, G18, or G19 is used.

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

D Distance moved and

feedrate for polar coordinate interpolation

The unit for coordinates on the hypothetical axis is the same as the unit for the linear axis (mm/inch)

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

D G codes which can be

specified in the polar coordinate interpolation mode

D Circular interpolation in

the polar coordinate plane

D Movement along axes

not in the polar coordinate interpolation plane in the polar coordinate interpolation mode

In the polar coordinate interpolation mode, program commands are specified with Cartesian coordinates on the polar coordinate interpolation plane. The axis address for the rotation axis is used as the axis address for the second axis (virtual axis) in the plane. Whether a diameter or radius is specified for the first axis in the plane is the same as for the rotation axis regardless of the specification for the first axis in the plane. The virtual axis is at coordinate 0 immediately after G12.1 is specified. Polar interpolation is started assuming the angle of 0 for the position of the tool when G12.1 is specified. Specify the feedrate as a speed (relative speed between the workpiece and tool) tangential to the polar coordinate interpolation plane (Cartesian coordinate system) using F.

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

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

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

G40, G41, G42 Cutter compensation . . .

(Polar coordinate interpolation is applied to the path

after cutter compensation.) G65, G66, G67 Custom macro command. . .

G90, G91 Absolute command, incremental command. . . . . . . .

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

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

⋅ I and J in the Xp–Yp plane when the linear axis is the X–axis or an axis

parallel to the X–axis.

⋅ J and K in the Y p–Zp plane when the linear axis is the Y–axis or an axis

parallel to the Y–axis.

⋅ K and I in the Zp–Xp plane when the linear axis is the Z–axis or an axis

parallel to the Z–axis.

The radius of an arc can be specified also with an R command. The tool moves along such axes normally, independent of polar

coordinate interpolation.

D Current position display

in the polar coordinate interpolation mode

Limitations

D Coordinate system for

the polar coordinate interpolation

D Tool offset command

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

Before G12.1 is specified, a local coordinate system (or workpiece coordinate system) where the center of the rotary axis is the origin of the coordinate system must be set. In the G12.1 mode, the coordinate system must not be changed (G92, G52, G53, relative coordinate reset, G54 through G59, etc.).

The polar coordinate interpolation mode cannot be started or terminated (G12.1 or G13.1) in the tool offset mode (G41 or G42). G12.1 or G13.1 must be specified in the tool offset canceled mode (G40).

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62764EN/01

D Tool length offset

command

D Tool offset command

D Program restart D Cutting feedrate for the

rotation axis

WARNING

T ool length of fset must be specified in the polar coordinate interpolation cancel mode before G12.1 is specified. It cannot be specified in the polar coordinate interpolation mode. Furthermore, no offset values can be changed in the polar coordinate interpolation mode.

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

For a block in the G12.1 mode, the program cannot be restarted. Polar coordinate interpolation converts the tool movement for a figure

programmed in a Cartesian coordinate system to the tool movement in the rotation axis (C–axis) and the linear axis (X–axis). When the tool moves closer to the center of the workpiece, the C–axis component of the feedrate becomes larger and may exceed the maximum cutting feedrate for the C–axis (set in parameter (No. 1422)), causing an alarm (see the figure below). To prevent the C–axis component from exceeding the maximum cutting feedrate for the C–axis, reduce the feedrate specified with address F or create a program so that the tool (center of the tool when cutter compensation is applied) does not move close to the center of the workpiece.

∆

θ1 θ2

θ3

L :Distance (in mm) between the tool center and workpiece center when the tool center is the nearest to the workpiece center R :Maximum cutting feedrate (deg/min) of the C axis Then, a speed specifiable with address F in polar coordinate interpolation can be given by the formula below. Specify a speed allowed by the formula. The formula provides a theoretical value; in practice, a value slightly smaller than a theoretical value may need to be used due to a calculation error.

L 1

F < L × R ×

Consider lines L1, L2, and L3. ∆X is the distance the tool moves per time unit

at the feedrate specified with address F in the Cartesian coordinate system. As the tool moves from L1 to L2 to L3, the angle at which the tool moves per

time unit corresponding to ∆X in the Cartesian coordinate system increases

fromθ1 toθ 2 to θ3.

In other words, the C–axis component of the feedrate becomes larger as the

tool moves closer to the center of the workpiece. The C component of the feedrate may exceed the maximum cutting feedrate for the C–axis because the tool movement in the Cartesian coordinate system has been converted to the tool movement for the C–axis and the X–axis.

(mm/min)

180

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

Examples

Example of Polar Coordinate Interpolation Program Based on X Axis(Linear Axis) and C Axis (Rotary Axis)

C’(hypothetical axis)

N204

N205

N206

C axis

N203

N202 N201

N208

N207

Path after cutter compensation

Program path

N200

X axis

Tool

Z axis

O0001 ;

N010 T0101

N0100 G90 G00 X60.0 C0 Z_ ; Positioning to start position N0200 G12.1 ; Start of polar coordinate interpolation N0201 G42 G01 X20.0 F_ ; N0202 C10.0 ; N0203 G03 X10.0 C20.0 R10.0 ; N0204 G01 X–20.0 ; Geometry program N0205 C–10.0 ; (program based on cartesian coordinates on N0206 G03 X–10.0 C–20.0 I10.0 J0 ; X–C’ plane) N0207 G01 X20.0 ; N0208 C0 ; N0209 G40 X60.0 ; N0210 G13.1 ; Cancellation of polar coordinate interpolation N0300 Z_ ; N0400 X_ C_ ;

N0900M30 ;

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62764EN/01

4.7

CYLINDRICAL INTERPOLATION (G07.1)

Format

The amount of travel of a rotary axis specified by an angle is once internally converted to a distance of a linear axis along the outer surface so that linear interpolation or circular interpolation can be performed with another axis. After interpolation, such a distance is converted back to the amount of travel of the rotary axis. The cylindrical interpolation function allows the side of a cylinder to be developed for programming. So programs such as a program for cylindrical cam grooving can be created very easily.

G07.1 IP r ; Starts the cylindrical interpolation mode

(enables cylindrical interpolation).

: :

G07.1 IP 0 ; The cylindrical interpolation mode is cancelled.

IP : An address for the rotation axis r : The radius of the cylinder

Specify G07.1 IP r ; and G07.1 IP 0; in separate blocks. G107 can be used instead of G07.1.

Explanations

D Plane selection

(G17, G18, G19)

D 

D Circular interpolation

(G02,G03)

Use parameter (No. 1022) to specify whether the rotation axis is the X–, Y–, or Z–axis, or an axis parallel to one of these axes. Specify the G code to select a plane for which the rotation axis is the specified linear axis. For example, when the rotation axis is an axis parallel to the X–axis, G17 must specify an Xp–Y p plane, which is a plane defined by the rotation axis and the Y–axis or an axis parallel to the Y–axis. Only one rotation axis can be set for cylindrical interpolation.

A feedrate specified in the cylindrical interpolation mode is a speed on the developed cylindrical surface.

In the cylindrical interpolation mode, circular interpolation is possible with the rotation axis and another linear axis. Radius R is used in commands in the same way as described in II–4.4. The unit for a radius is not degrees but millimeters (for metric input) or inches (for inch input). < Example Circular interpolation between the Z axis and C axis >

For the C axis of parameter (No.1022), 5 (axis parallel with the X axis) is to be set. In this case, the command for circular interpolation is

G18 Z__C__;

G02 (G03) Z__C__R__; For the C axis of parameter (No.1022), 6 (axis parallel with the Y axis) may be specified instead. In this case, however, the command for circular interpolation is

G19 C__Z__;

G02 (G03) Z__C__R__;

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

D Tool offset

D Cylindrical interpolation

accuracy

To perform tool offset in the cylindrical interpolation mode, cancel any ongoing cutter compensation mode before entering the cylindrical interpolation mode. Then, start and terminate tool offset within the cylindrical interpolation mode.

In the cylindrical interpolation mode, the amount of travel of a rotary axis specified by an angle is once internally converted to a distance of a linear axis on the outer surface so that linear interpolation or circular interpolation can be performed with another axis. After interpolation, such a distance is converted back to an angle. For this conversion, the amount of travel is rounded to a least input increment. So when the radius of a cylinder is small, the actual amount of travel can differ from a specified amount of travel. Note, however, that such an error is not accumulative. If manual operation is performed in the cylindrical interpolation mode with manual absolute on, an error can occur for the reason described above.

The actual amount of travel

MOTION REV

2×2πR

The amount of travel per rotation of the rotation axis (Set-

ting value of parameter No. 1260)

Workpiece radius



Specified value

2×2πR



MOTION REV

Limitations

D Arc radius specification

in the cylindrical interpolation mode

D Circular interpolation

and cutter compensation

D Positioning

D Coordinate system

setting

D Cylindrical interpolation

mode setting

:Rounded to the least input increment

In the cylindrical interpolation mode, an arc radius cannot be specified with word address I, J, or K.

If the cylindrical interpolation mode is started when cutter compensation is already applied, circular interpolation is not correctly performed in the cylindrical interpolation mode.

In the cylindrical interpolation mode, positioning operations (including those that produce rapid traverse cycles such as G28, G53, G73, G74, G76, G80 through G89) cannot be specified. Before positioning can be specified, the cylindrical interpolation mode must be cancelled. Cylindrical interpolation (G07.1) cannot be performed in the positioning mode (G00).

In the cylindrical interpolation mode, a workpiece coordinate system (G92, G54 through G59) or local coordinate system (G52) cannot be specified.

In the cylindrical interpolation mode, the cylindrical interpolation mode cannot be reset. The cylindrical interpolation mode must be cancelled before the cylindrical interpolation mode can be reset.

D Tool offset

D Index table indexing

function

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

Cylindrical interpolation cannot be specified when the index table index function is being used.

4. INTERPOLA TION FUNCTIONS

Examples

PROGRAMMING

B–62764EN/01

Example of a Cylindrical Interpolation Program

O0001 (CYLINDRICAL INTERPOLATION ); N01 G00 G90 Z100.0 C0 ; N02 G01 G91 G18 Z0 C0 ; N03 G07.1 C57299 ; N04 G90 G01 G42 Z120.0 D01 F250 ; N05 C30.0 ; N06 G02 Z90.0 C60.0 R30.0 ; N07 G01 Z70.0 ; N08 G03 Z60.0 C70.0 R10.0 ; N09 G01 C150.0 ; N10 G03 Z70.0 C190.0 R75.0 ; N11 G01 Z110.0 C230.0 ; N12 G02 Z120.0 C270.0 R75.0 ; N13 G01 C360.0 ; N14 G40 Z100.0 ; N15 G07.1 C0 ; N16 M30 ;

120 110

70 60

N05

N06

N11

N07

N08 N09 N10

60 70

150

N12

230190

270

N13

360

deg

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.8 INVOLUTE INTERPOLATION (G02.2, G03.2)

Involute curve machining can be performed by using involute interpolation. Involute interpolation ensures continuous pulse distribution even in high–speed operation in small blocks, thus enabling smooth and high–speed machining. Furthermore, machining tapes can be created easily and efficiently, reducing the required length of tape.

4. INTERPOLA TION FUNCTIONS

Format

PROGRAMMING

Involute interpolation on the X–Y plane

G17 G02.2 X__Y__I__J__R__F__ ; G17 G03.2 X__Y__I__J__R__F__ ;

Involute interpolation on the Z–X plane

G18 G02.2 Z_ G18 G03.2 Z_

X__K__I__R__F__ ; X__K__I__R__F__ ;

Involute interpolation on the Y–Z plane

G19 G02.2 Y__Z__J__K__R__F__ ; G19 G03.2 Y__Z__J__K__R__F__ ;

Where, G02.2: Involute interpolation (clockwise) G03.2: Involute interpolation (counterclockwise) G17/G18/G19 : X –Y / Z–X / Y–Z plane selection X, Y, Z : Involute curve end coordinate I, J, K : Center of the base circle for an involute curve viewed

from the start point R : Base circle radius F : Cutting feedrate

Yp Yp

B–62764EN/01

Start point

Base circle

P e

End point

Clockwise involute interpolation (G02.2)

End point

Start point

Ps Po

Xp Xp

Counterclockwise involute interpolation (G03.2)

B–62764EN/01

Explanations

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

D Involute curve

An involute curve on the X–Y plane is defined as follows ;

X (θ)=R [cos θ+ (θ-θ0 ) sin θ] +X

Y (θ)=R [sin θ- (θ-θ0 ) cos θ] +Y

where,

X0 , Y0: Coordinates of the center of a base circle R:Base circle radius

θ0: Angle of the start point of an involute curve θ : Angle of the point where a tangent from the current position

to the base circle contacts the base circle

X (θ), Y (θ): Current position on the X–axis and Y–axis

Involute curve

Start point

(X,Y)

θ0

(X0,Y0)

Base circle

End point

D Start point and end point

D Base circle specification

Fig.4.8 (a) Involute Curve

Involute curves on the Z–X plane and Y–Z plane are defined in the same way as an involute curve on the X–Y plane.

The end point of an involute curve is specified using address X, Y, or Z. An absolute value or incremental value is used to specify an X, Y, or Z value. When using an incremental value, specify the coordinates of the end point viewed from the start point of the involute curve. When no end point is specified, P/S alarm No. 241 is issued. If the specified start point or end point lies within the base circle, P/S alarm No. 242 is issued. The same alarm is issued if cutter compensation C causes the offset vector to enter the base circle. Be particularly careful when applying an offset to the inside of an involute curve.

The center of a base circle is specified with I, J, and K, corresponding to X, Y, and Z. The value following I, J, or K is a vector component defined when the center of the base circle is viewed from the start point of the involute curve; this value must always be specified as an incremental value, regardless of the G90/G91 setting. Assign a sign to I, J, and K according to the direction. If I, J, and K are all left unspecified, or I0J0K0 is specified, P/S alarm No. 241 or No. 242 is issued. If R is not specified, or R < 0, P/S alarm No. 241 or No. 242 is issued.

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62764EN/01

D Choosing from two types

of involute curves

D Feedrate

D Plane selection

D Cutter compensation C

When only a start point and I, J, and K data are given, two types of involute curves can be created. One type of involute curve extends towards the base circle, and the other extends away from the base circle. When the specified end point is closer to the center of the base circle than the start point, the involute curve extends toward the base circle. In the opposite case, the involute curve extends away from the base circle.

The cutting feedrate specified in an F code is used as the feedrate for involute interpolation. The feedrate along the involute curve (feedrate along the tangent to the involute curve) is controlled to satisfy the specified feedrate.

As with circular interpolation, the plane to which to apply involute interpolation can be selected using G17, G18, and G19.

Cutter compensation C can be applied to involute curve machining. As with linear and circular interpolation, G40, G41, and G42 are used to specify cutter compensation.

G40 : Cutter compensation cancel G41 : Cutter compensation left G42 : Cutter compensation right

Cutter compensation for an involute curve is implemented as described below. First, near the start point of an involute curve, an arc with a curvature close to the curvature of the involute curve is found. Next, an offset intersection between the arc and the linear line or arc in the previous block is found. Similarly, an offset intersection is found near the end point. Then, the involute curve passing through the two points is used as the tool center path. In involute interpolation mode, cutter compensation cannot be started or cancelled.

Tool center path

Programmed path

Start point

Arc with a curvature closer to the curvature of the involute curve near the start point

Arc with a curvature closer to the curvature of the involute curve near the end point

End point

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

D Specifiable G codes

D Modes that allow

involute interpolation specification

D End point error

The following G codes can be specified in involute interpolation mode:

G04 : Dwell G10 : Data setting G17 : X–Y plane selection G18 : Z–X plane selection G19 : Y–Z plane selection G65 : Macro call G66 : Macro modal call G67 : Macro modal call cancel G90 : Absolute command G91 : Incremental command

Involute interpolation can be specified in the following G code modes:

G41 : Cutter compensation left G42 : Cutter compensation right G51 : Scaling G51.1 : Programmable mirror image G68 : Coordinate rotation

As shown below the end point may not be located on an involute curve that passes through the start point. When an involute curve that passes through the start point deviates from the involute curve that passes through the end point by more than the value set in parameter No. 5610, P/S alarm No. 243 is issued. When there is an end point error, the feedrate is not guaranteed.

End point

Deviation

Fig. 4.8 (b) End Point Error in Counterclockwise Involute Interpolation (G03.2)

Path after correction

Start point

Correct involute curve

4. INTERPOLA TION FUNCTIONS

Limitations

PROGRAMMING

B–62764EN/01

D Number of involute curve

turns

D Unspecifiable functions

D Modes that do not allow

involute interpolation specification

D Cutting accuracy

Both the start point and end point must be within 100 turns from the point where the involute curve starts. An involute curve can be specified to make one or more turns in a single block. If the specified start point or end point is beyond 100 turns from the point where the involute curve starts, P/S alarm No. 242 is issued.

In involute interpolation mode, chamfer corner R (with an arbitrary angle), helical cutting, or axis–by–axis scaling functions cannot be specified.

Involute interpolation cannot be used in the following modes:

G41.1 (G151) : Normal direction control left side on G42.1 (G152) : Normal direction control right side on G07.1 (G107) : Cylindrical interpolation G12.1 : Polar coordinate interpolation mode G16 : Polar coordinates command G72.1 : Drawing copy

The curvature of an involute curve varies rather sharply near the base circle. In such locations, a larger load is applied to the cutter when the programmed feedrate is used for cutting; in this case, the surface produced may be somewhat uneven

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.9

EXPONENTIAL INTERPOLATION (G02.3, G03.3)

Exponential interpolation exponentially changes the rotation of a workpiece with respect to movement on the rotary axis. Furthermore, exponential interpolation performs linear interpolation with respect to another axis. This enables tapered groove machining with a constant helix angle (constant helix taper machining). This function is best suited for grooving and grinding tools such as end mills.

β2β

X (Linear axis)

Helix angle

= β2= β

Format

X

A (Rotary axis)

A

positive rotation (ω=0)

G02. 3 X__ Y__ Z__ I__ J__ K__ R__ F__ Q__ ;

Negative rotation (ω=1)

G03. 3 X__ Y__ Z__ I__ J__ K__ R__ F__ Q__ ;

X__; Specifies an end point with an absolute or incremental value. Y__; Specifies an end point with an absolute or incremental value. Z__; Specifies an end point with an absolute or incremental value. I__ ; Specifies angl I (from 1to 89 deg in units of 0.001deg ). J__ ; Specifies angle J (from 1 to 89 degin units of 0.001deg). K__; Specifies the amount to divide the linear axis for exponential

interpolation (span value). Specify a positive value. When no value is specified, the value specified in parameter

(No. 5643) is used. R__; Specifies constant R for exponential interpolation. F__; Specifies the initial feedrate.

Specified in the same way as an ordinary F code. Specify a

composite feedrate including a feedrate on the rotary axis. Q__ ; Specifies the feedrate at the end point.

The same unit used for F is used. The CNC internally performs interpolation between the initial feedrate (F) and final feedrate (Q), depending on the travel distance on the linear axis.

4. INTERPOLA TION FUNCTIONS

Explanations

PROGRAMMING

B–62764EN/01

D Exponential relational

expressions

Exponential relational expressions for a linear axis and rotary axis are defined as follows:

X(θ)=R  (e –1)  A()=(–1)360

tan (I)

2π

⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅

Movement on the linear axis (1)

Movement on the linear axis (2)

Where,

tan (J)

K =

tan (I)

ω=0/1 ⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅

R, I, and J are constants, and θ represents an angle (radian)

Rotation direction

The following is obtained from Expression (1)

(X)=Kln( +1)

Xtan (I)

When there is movement from X1 to X2 on the linear axis, the amount of movement on the rotary axis is determined by :

tan (I)

= K{ ln ( +1) – ln ( +1)}

tan (I)



Specify Expressions (1) and (2) in the format described earlier.

X (linear axis)

Limitations

D Cases where linear

interpolation is performed

D Tool length

compensation / cutter compensation

X

A (rotary axis)

A

Even when the G02.3 or G03.3 mode is set, linear interpolation is performed in the following cases: S When the linear axis specified in parameter( No. 5641) is not specified,

or the amount of movement on the linear axis is 0

S When the rotary axis specified in parameter (No. 5642) is specified S When the amount for dividing the linear axis (span value) is 0

Neither tool length compensation nor cutter compensation can be used in the G02.3 and G03.3 modes.

B–62764EN/01

Examples

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

CAUTION

The amount for dividing the linear axis for exponential interpolation (span value) affects figure precision. However , if an excessively small value is set, the machine may stop during interpolation. Try to specify an optimal span value depending on the machine being used.

Constant helix machining for producing a tapered figure

Constant helix machining for producing a reverse tapered figure

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62764EN/01

Relational expressions

Z (θ) = { –Utan (I) }(e –1) +Z (0) (3)

X (θ) = { –Utan (I) }(e –1) (4) A () = (–1)360

2π

tan (B) tan (I)

tan (I)

⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅

⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅

where

tan (J)

K =

tan (I)

X (), Z (), A (): Absolute value on the X–axis, Z–axis, and

A–axis from the origin r : Left end diameter U : Excess length I : T aper angle B : Groove bottom taper angle J : Helix angle X : Amount of movement on the linear axis

 : Helix direction (0: Positive, 1: Negative)  : Workpiece rotation angle

From expressions (3) and (4), the following is obtained ;

Z () = tan (B)  X () + Z (0) (5)

⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅

The groove bottom taper angle (B) is determined from the end point position on the X–axis and Z–axis according to Expression

5. The amount of movement on the Z–axis is determined from a groove bottom taper angle (B) and X–axis position.

From Expressions (1) and (4), the following is determined:

R = r/2 – Utan (I) (6)

⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅

Constant R is determined from the left end diameter (r) and excess length (U) according to Expression (6). Specify a taper angle (I) in address I, and specify a helix angle (J) in address J. Note, however, that a negative value must be specified as the taper angle (I) for constant helix machining in order to produce a reverse tapered figure. Select a helix direction with G02.3 or G03.3. The user can perform constant helix machining to produce a tapered figure or a reverse tapered figure.

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.10 SMOOTH INTERPOLATION (G05.1)

Format

Either of two types of machining can be selected, depending on the program command.

D For those portions where the accuracy of the figure is critical, such as

at corners, machining is performed exactly as specified by the program command.

D For those portions having a large radius of curvature where a smooth

figure must becreated, points along the machining path are interpolated with a smooth curve, calculated from the polygonal lines specified with the program command (smooth interpolation).

Smooth interpolation can be specified when CDSP (bit 5 of parameter No.

8485) is set to 1 in high–speed contour control mode (between G05 P10000 and G05 P0). Smooth interpolation performed in high–speed contour control mode is described below. For details of high–speed contour control, see Section 20.5.

Starting of smooth interpolation mode

G05.1 Q2X0Y0Z0;

Cancelation of smooth interpolation mode

Explanations

D Characteristics of

smooth interpolation

G05.1 Q 0;

To machine a part having sculptured surfaces, such as metal moldings used in automobiles and airplanes, a part program usually approximates the sculptured surfaces with minute line segments. As shown in the following figure, a sculptured curve is normally approximated using line segments with a tolerance of about 10 m.

Enlarged

10 m

: Specified point

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62764EN/01

When a program approximates a sculptured curve with line segments, the length of each segment differs between those portions that have mainly a small radius of curvature and those that have mainly a large radius of curvature. The length of the line segments is short in those portions having a small radius of curvature, while it is long in those portions having a large radius of curvature. The high–precision contour control of the FANUC Series 15 moves the tool along a programmed path thus enabling highly precise machining. This means that the tool movement precisely follows the line segments used to approximate a sculptured curve. This may result in a non–smooth machined curve if control is applied to machining a curve where the radius of curvature is large and changes only gradually . Although this effect is caused by high–precision machining, which precisely follows a pre–programmed path, the uneven corners that result will be judged unsatisfactory when smooth surfaces are required.

Profile Portions having

mainly a small radius

of curvature

Example of machined parts

Length of line segment Short Long Resulting surfaces pro-

duced using high–precision contour control

Automobile parts Decorative parts, such

Smooth surface even when machining is performed exactly as specified by a program

mainly a large radius

as body side moldings

Uneven surfaces may result when machining is performed exactly as specified by a program

Portions having

of curvature

Example of uneven surfaces (polygon) resulting from machining that precisely follows the line segments.

In smooth interpolation mode, the CNC automatically determines, according to the program command, whether an accurate figure is required, such as at corners, or a smooth figure is required where the radius of curvature is large. If a block specifies a travel distance or direction which differs greatly from that in the preceding block, smooth interpolation is not performed for that block. Linear interpolation is performed exactly as specified by the program command. Programming is thus very simple.

B–62764EN/01

Examples

N17

PROGRAMMING

Interpolated by smooth curve

4. INTERPOLA TION FUNCTIONS

Linear interpolation

D Conditions for

performing smooth interpolation

N17

N16

N15

N14

Interpolated by smooth curve

N15

N14

N13

N12

N11

N10

Linear interpolation

N11

N10

Smooth interpolation is performed when all the following conditions are satisfied. If any of the following conditions is not satisfied for a block, that block is executed without smooth interpolation then the conditions are checked for the next block.

D Commands which cancel

smooth interpolation

(1)The machining length specified in the block is shorter than the length

specified with parameter No. 8486. (2)The machining length is other than 0. (3)The modes are:

G01 : Linear interpolation

G13.1 : Polar coordinate interpolation cancel

G15 : Polar coordinate command cancel

G40 : Cutter compensation cancel

(except for 3–dimensional tool compensation) G64 : Cutting mode G80 : Canned cycle cancel G94 : Feed per minute

(4)Machining is specified only along the axes specified with G05.1Q2. (5) The block is judged to be unsuitable for smooth interpolation, as

performed with the internal algorithm of the CNC.

(1)Auxiliary and second auxiliary functions (2)M98, M99 : Subprogram call

M198 : Calling a subprogram in external memory

4. INTERPOLA TION FUNCTIONS

Limitations

PROGRAMMING

B–62764EN/01

D Controlled axes

D High–precision contour

control mode

Examples

Smooth interpolation can be specified only for the X–, Y–, and Z–axes and any axes parallel to these axes (up to three axes at one time).

Commands for turning on and off smooth interpolation mode must be executed in high–precision contour control mode.

Example program for smooth interpolation

G05 P10000 ; N10 X–1000 Z350 ; . N11 X–1000 Z175 ; . N12 X–1000 Z25 ; G91 ; N13 X–1000 Z– 50 ; G05. 1 Q2 X0 Y0 Z0 ; N14 X–1000 Z– 50 ; N01 G01 X1000 Z–300 ; N15 X–1000 Z50 ; N02 X1000 Z–200 ; N16 X–1000 Z200 ; N03 X1000 Z–50 ; N17 X–1000 Z300 ; N04 X1000 Z50 ; G05. 1 Q0 ; N05 X1000 Z50 ; . N06 X1000 Z–25 ; . N07 X1000 Z–175 ; G05 P0 ; N08 X1000 Z–350 ; . N09 Y1000 ; .

N17

N16

Interpolated by smooth curve

N13

N15

N14

N12

N11

N10

Linear interpolation

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.11 HYPOTHETICAL AXIS INTERPOLATION (G07)

Format

Explanations

D Sine interpolation

In helical interpolation, when pulses are distributed with one of the circular interpolation axes set to a hypothetical axis, sine interpolation is enabled. When one of the circular interpolation axes is set to a hypothetical axis, pulse distribution causes the speed of movement along the remaining axis to change sinusoidally. If the major axis for threading (the axis along which the machine travels the longest distance) is set to a hypothetical axis, threading with a fractional lead is enabled. The axis to be set as the hypothetical axis is specified with G07.

G07  0; Hypothetical axis setting G07  1; Hypothetical axis cancel

Where,  is any one of the addresses of the controlled axes.

The  axis is regarded as a hypothetical axis for the period of time from the G07  0 command until the G07  1 command appears. Suppose sine interpolation is performed for one cycle in the YZ plane. The hypothetical axis is then the X axis.

+ Y2 = r2 (r is the radius of an arc.)

Y = r SIN (

2

Z )

(1 is the distance traveled along the Z–axis in one cycle.)

D Interlock, stroke limit,

and external deceleration

D Handle interrupt



 2

Interlock, stroke limit, and external deceleration can also apply to the hypothetical axis.

An interrupt caused by the handle also applies to the hypothetical axis. This means that movement for a handle interrupt is performed.

4. INTERPOLA TION FUNCTIONS

Limitations

PROGRAMMING

B–62764EN/01

D Manual operation

D Move command D Coordinate rotation

Examples

D Sine interpolation

The hypothetical axis can be used only in automatic operation. In manual operation, it is not used, and movement takes place.

Specify hypothetical axis interpolation only in the incremental mode. Hypothetical axis interpolation does not support coordinate rotation.

10.0

20.0

D Changing the feedrate to

form a sine curve

N001 G07 X0 ; N002 G91 G17 G03 X–20.2 Y0.0 I–10.0 Z20.0 F100 ; N003 G01 X10.0 ; N004 G07 X1 ; From the N002 to N003 blocks, the X–axis is set to a hypothetical axis. The N002 block specifies helical cutting in which the Z–axis is the linear axis. Since no movement takes place along the X axis, movement along the Y–axis is performed while performing sine interpolation along the Z–axis. In the N003 block, there is no movement along the X–axis, and so the machine dwells until interpolation terminates.

(Sample program) G07Z0 ; The Z–axis is set to a hypothetical axis. G02X0Z0I10.0F4. ; The feedrate on the X–axis changes sinusoidally. G07Z1 ; The use of the Z–axis as a hypothetical axis is

canceled.

4.0

B–62764EN/01

Inch i

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.12

THREAD CUTTING (G33)

Format

Explanations

Straight threads with a constant lead can be cut. The position coder mounted on the spindle reads the spindle speed in real–time. The read spindle speed is converted to the feedrate per minute to feed the tool.

G33 _ F_ ; F : Long axis direction lead



In general, thread cutting is repeated along the same tool path in rough cutting through finish cutting for a screw . Since thread cutting starts when the position coder mounted on the spindle outputs a 1–turn signal, threading is started at a fixed point and the tool path on the workpiece is unchanged for repeated thread cutting. Note that the spindle speed must remain constant from rough cutting through finish cutting. If not, incorrect thread lead will occur. 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 thread cutting length somewhat longer than required should be specified. Table 4.12 (a) lists the ranges for specifying the thread lead.

T able. 4.12 (a) Ranges of lead sizes that can be specified

mm inpu

npu

Least command

increment

0.001 mm F1 to F50000 (0.01 to 500.00mm)

0.0001 mm F1 to F50000 (0.01 to 500.00mm)

0.0001 inch F1 to F99999

0.00001 inch F1 to F99999

Command value range of the lead

(0.0001 to 9.9999inch)

4. INTERPOLA TION FUNCTIONS

NOTE

1 The spindle speed is limited as follows :

PROGRAMMING

B–62764EN/01

1  spindle speed 

Maximum feedrate

Thread lead

Spindle speed : rpm Thread lead : mm or inch Maximum feedrate : mm/min or inch/min ; maximum command–specified feedrate for feed–per–minute mode or maximum feedrate that is determined based on mechanical restrictions including those related to motors, whichever is smaller

2 Cutting feedrate override is not applied to the converted feedrate in all machining process from

rough cutting to finish cutting. The feedrate is fixed at 100% 3 The converted feedrate is limited by the upper feedrate specified. 4 Feed hold is disabled during threading. Pressing the feed hold key during thread cutting causes

the machine to stop at the end point of the next block after threading (that is, after the G33 mode

is terminated)

Examples

Thread cutting at a pitch of 1.5mm

G33 Z10. F1.5;

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.13

SKIP FUNCTION(G31)

Format

Explanations

Linear interpolation can be commanded by specifying axial move following the G31 command, like G01. If an external skip signal is input during the execution of this command, execution of the command is interrupted and the next block is executed. The skip function is used when the end of machining is not programmed but specified with a signal from the machine, for example, in grinding. It is used also for measuring the dimensions of a workpiece.

G31 IP_ ; G31: One–shot G code (If is effective only in the block in which it

is specified)

The coordinate values when the skip signal is turned on can be used in a custom macro because they are stored in the custom macro system variable #5061 to #5064, as follows:

#5061 X axis coordinate value #5062 Y axis coordinate value #5063 Z axis coordinate value #5064 4th axis coordinate value #5065 5th axis coordinate value #5066 6th axis coordinate value #5067 7th axis coordinate value #5068 8th axis coordinate value

WARNING

Disable feedrate override, dry run, and automatic acceleration/deceleration (however, these become available by setting the parameter SKF No.6200#7 to 1.) when the feedrate per minute is specified, allowing for an error in the position of the tool when a skip signal is input. These functions are enabled when the feedrate per rotation is specified.

NOTE

If G31 command is issued while cutter compensation C is applied, an P/S alarm of No.035 is displayed. Cancel the cutter compensation with the G40 command before the G31 command is specified.

4. INTERPOLA TION FUNCTIONS

Examples D The next block to G31 is

an incremental command

PROGRAMMING

G31 G91X100.0 F100;

Y50.0;

B–62764EN/01

D The next block to G31 is

an absolute command for 1 axis

Skip signal is input here

100.0

Fig.4.13 (a) The next block is an incremental command

G31 G90X200.00 F100;

Y100.0;

Skip signal is input here

Y100.0

50.0

Actual motion Motion without skip signal

X200.0

D The next block to G31 is

an absolute command for 2 axes

Actual motion Motion without skip signal

Fig.4.13 (b) The next block is an absolute command for 1 axis

G31 G90X200.0 F100;

X300.0 Y100.0; Y

Skip signal is input here

100

100 200 300

Fig 4.13 (c) The next block is an absolute command for 2 axes

(300,100)

Actual motion Motion without skip signal

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.14 MULTISTAGE SKIP (G31)

Format

In a block specifying P1 to P4 after G31, the multistage skip function stores coordinates in a custom macro variable when a skip signal (4–point or 8–point ; 8–point when a high–speed skip signal is used) is turned on. Parameters No. 6202 to No. 6205 can be used to select a 4–point or 8–point (when a high–speed skip signal is used) skip signal. One skip signal can be set to match multiple Pn or Qn (n=1,2,3,4) as well as to match a Pn or Qn on a one–to–one basis. Parameters DS1 to DS8 (No. 6206 #0A#7) can be used for dwell. A skip signal from equipment such as a fixed–dimension size measuring instrument can be used to skip programs being executed. In plunge grinding, for example, a series of operations from rough machining to spark–out can be performed automatically by applying a skip signal each time rough machining, semi–fine machining, fine–machining, or spark–out operation is completed.

Move command

G31 IP __ F __ P __ ;

IP_ : End point

F_ : Feedrate P_ : P1–P4

Explanations

D Correspondence to skip

signals

Dwell

G04 X (U, P)__ (Q__) ;

X(U, P)_ : Dwell time Q_ : Q1 – Q4

Multistage skip is caused by specifying P1, P2, P3, or P4 in a G31 block. For an explanation of selecting (P1, P2, P3, or P4), refer to the manual supplied by the machine tool builder. Specifying Q1, Q2, Q3, or Q4 in G04 (dwell command) enables dwell skip in a similar way to specifying G31. A skip may occur even if Q is not specified. For an explanation of selecting (Q1, Q2, Q3, or Q4), refer to the manual supplied by the machine tool builder.

Parameter Nos. 6202 to 6205 can be used to specify whether the 4–point or 8–point skip signal is used (when a high–speed skip signal is used). Specification is not limited to one–to–one correspondence. It is possible to specify that one skip signal correspond to two or more Pn’s or Qn’s (n=1, 2, 3, 4). Also, bits 0 (DS1) to 7 (DS8) of parameter No. 6206 can be used to specify dwell.

CAUTION

Dwell is not skipped when Qn is not specified and parameters DS1–DS8 (No. 6206#0–#7) are not set.

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62764EN/01

4.15 HIGH SPEED SKIP SIGNAL (G31)

Format

The skip function operates based on a high–speed skip signal (connected directly to the NC; not via the PMC) instead of an ordinary skip signal. In this case, up to eight signals can be input. Delay and error of skip signal input is 0 – 2 msec at the NC side (not considering those at the PMC side). This high–speed skip signal input function keeps this value to 0.1 msec or less, thus allowing high precision measurement.

For details, refer to the appropriate manual supplied from the machine tool builder.

G31 IP_ ;

G31: One–shot G code (If is effective only in the block in which it is

specified)

B–62764EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.16 CONTINUOUS HIGH–SPEED SKIP FUNCTION (G31)

Format

Explanations

D Custom macro variables

The continuous high–speed skip function enables reading of absolute coordinates by using the high–speed skip signal. Once a high–speed skip signal has been input in a G31P90 block, absolute coordinates are read into custom macro variables #5061 to #5068. The input of a skip signal does not stops axial movement, thus enabling reading of the coordinates of two or more points.

The rising and falling edges of the high–speed skip signal can be used as a trigger, depending on the parameter BHIS (No. 6201#5) setting.

G31 P90 __ F__

__: Skip axis address and amount of travel

Only one axis can be specified. G31 is a one–shot G code.

Once a high–speed skip signal has been input in a G31P90 block, absolute coordinates are read into custom macro variables #5061 to #5068. These variables are immediately updated once the tool reaches the next skip position. The feedrate must, therefore, be specified such that the tool does not reach the next skip position before the application completes reading of the variables. For details of the application, refer to the appropriate manual supplied from the machine tool builder.

D High–speed skip signal

D End of block

Limitations

D Controlled axes

#5061 Coordinate along the first axis #5062 Coordinate along the second axis #5063 Coordinate along the third axis



#5068 Coordinate along the eighth axis This function is enabled only when a high–speed skip signal is used. The high–speed skip signal to be used is selected with bits 0 to 7 of

parameter No. 6208 (9S1 to 9S8). The G31P90 block is terminated when the tool reaches the end point.

Only one axis can be specified in the block for the continuous high–speed skip function (G31P90). If two or more axes are specified, P/S alarm No. 5068 is issued.

fanuc 16C, 160C, 18C, 180-C Operators Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

SAFETY PRECAUTIONS

GENERAL WARNINGS AND CAUTIONS

Table of Contents

Related manuals

NOTES ON READING THIS MANUAL

Coordinate system

PROGRAM CONFIGURATION

TOOL FIGURE AND TOOL MOTION BY PROGRAM

CONTROLLED AXES

Increment system Maximum stroke

INTERPOLATION FUNCTIONS

POSITIONING (G00)

SINGLE DIRECTION POSITIONING (G60)

THREAD CUTTING (G33)

SKIP FUNCTION(G31)