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

Download

GE Fanuc Automation

Computer Numerical Control Products

Series 16 / 18 / 160 / 180 – Model C for Lathe

Operator's Manual

B-62754EN/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–62754EN/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–62754EN/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–62754EN/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–62754EN/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–62754EN/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–62754EN/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–62754EN/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–62754EN/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–62754EN/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–62754EN/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–62754EN/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 15. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.3 PART DRAWING AND TOOL MOVEMENT 16. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.3.1 Reference Position (Machine–Specific Position) 16. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.3.2 Coordinate System on Part Drawing and Coordinate System Specified by CNC – Coordinate System 17. . .

1.3.3 How to Indicate Command Dimensions for Moving the Tool – Absolute, Incremental Commands 20. . . . . .

1.4 CUTTING SPEED – SPINDLE SPEED FUNCTION 23. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.5 SELECTION OF TOOL USED FOR VARIOUS MACHINING – TOOL FUNCTION 24. . . . . . . . . . .

1.6 COMMAND FOR MACHINE OPERATIONS – MISCELLANEOUS FUNCTION 25. . . . . . . . . . . . .

1.7 PROGRAM CONFIGURATION 26. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.8 TOOL FIGURE AND TOOL MOTION BY PROGRAM 29. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.9 TOOL MOVEMENT RANGE – STROKE 30. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2. CONTROLLED AXES 31. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1 CONTROLLED AXES 32. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.2 NAMES OF AXES 33. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3 INCREMENT SYSTEM 34. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4 MAXIMUM STROKES 35. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3. PREPARATORY FUNCTION (G FUNCTION) 36. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4. INTERPOLATION FUNCTIONS 41. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.1 POSITIONING (G00) 42. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.2 LINEAR INTERPOLATION (G01) 44. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

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

4.5 POLAR COORDINATE INTERPOLATION (G12.1, G13.1) 50. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

4.7 HYPOTHETICAL AXIS INTERPOLATION (G07) 57. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8 CONSTANT LEAD THREADING (G32) 59. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.9 VARIABLE–LEAD THREAD CUTTING (G34) 63. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.10 CONTINUOUS THREAD CUTTING 64. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.11 MULTIPLE–THREAD CUTTING 65. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–1

T ABLE OF CONTENTS

4.12 CIRCULAR THREADING (G35, G36) 67. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.13 SKIP FUNCTION (G31) 70. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.14 MULTISTAGE SKIP 72. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.15 TORQUE LIMIT SKIP (G31 P99) 73. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–62754EN/01

5. FEED FUNCTIONS 75. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.1 GENERAL 76. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.2 RAPID TRAVERSE 78. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.3 CUTTING FEED 79. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4 DWELL (G04) 82. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6. REFERENCE POSITION 83. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7. FLOATING REFERENCE POSITION RETURN (G30.1) 86. . . . . . . . . . . . . . . . . . . . . . . . .

8. COORDINATE SYSTEM 87. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1 MACHINE COORDINATE SYSTEM 88. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2 WORKPIECE COORDINATE SYSTEM 89. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2.1 Setting a Workpiece Coordinate System 89. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2.2 Selecting a Workpiece Coordinate System 91. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2.3 Changing Workpiece Coordinate System 92. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2.4 Workpiece Coordinate System Preset (G92.1) 94. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2.5 Workpiece Coordinate System shift 96. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3 LOCAL COORDINATE SYSTEM 97. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4 PLANE SELECTION 99. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9. COORDINATE VALUE AND DIMENSION 100. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1 ABSOLUTE AND INCREMENTAL PROGRAMMING (G90, G91) 101. . . . . . . . . . . . . . . . . . . . . . . .

9.2 INCH/METRIC CONVERSION (G20, G21) 102. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3 DECIMAL POINT PROGRAMMING 103. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4 DIAMETER AND RADIUS PROGRAMMING 104. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.SPINDLE SPEED FUNCTION 105. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.1 SPECIFYING THE SPINDLE SPEED WITH A CODE 106. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2 SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY (S5–DIGIT COMMAND) 106. . . . . . . . .

10.3 CONSTANT SURFACE SPEED CONTROL (G96, G97) 106. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.4 SPINDLE SPEED FLUCTUATION DETECTION FUNCTION (G25, G26) 110. . . . . . . . . . . . . . . . . .

10.5 SPINDLE POSITIONING FUNCTION 113. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.5.1 Spindle Orientation 113. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.5.2 Spindle Positioning 113. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.5.3 Canceling Spindle Positioning 115. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.TOOL FUNCTION (T FUNCTION) 116. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1 TOOL SELECTION 117. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2 TOOL LIFE MANAGEMENT 118. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.1 Program of Tool Life Data 118. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.2 Counting a Tool Life 121. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.3 Specifying a Tool Group in a Machining Program 122. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–2

B–62754EN/01

T ABLE OF CONTENTS

12.AUXILIARY FUNCTION 123. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.1 AUXILIARY FUNCTION (M FUNCTION) 124. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.2 MULTIPLE M COMMANDS IN A SINGLE BLOCK 125. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.3 M CODE GROUP CHECK FUNCTION 126. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.4 THE SECOND AUXILIARY FUNCTIONS (B CODES) 127. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.PROGRAM CONFIGURATION 128. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1 PROGRAM COMPONENTS OTHER THAN PROGRAM SECTIONS 130. . . . . . . . . . . . . . . . . . . . .

13.2 PROGRAM SECTION CONFIGURATION 133. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.3 SUBPROGRAM 139. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.4 8–DIGIT PROGRAM NUMBER 142. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.FUNCTIONS TO SIMPLIFY PROGRAMMING 145. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1 CANNED CYCLE (G90, G92, G94) 146. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.1 Outer Diameter / Internal Diameter Cutting Cycle (G90) 146. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.2 Thread Cutting Cycle (G92) 148. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.3 End Face Turning Cycle (G94) 151. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.4 How to Use Canned Cycles (G90, G92, G94) 154. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2 MULTIPLE REPETITIVE CYCLE (G70–G76) 156. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2.1 Stock Removal in Turning (G71) 156. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2.2 Stock Removal In Facing (G72) 160. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2.3 Pattern Repeating (G73) 161. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2.4 Finishing Cycle (G70) 162. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2.5 End Face Peck Drilling Cycle (G74) 166. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2.6 Outer Diameter / Internal Diameter Drilling Cycle (G75) 167. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2.7 Multiple Thread Cutting Cycle (G76) 168. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2.8 Notes on Multiple Repetitive Cycle (G70–G76) 172. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3 CANNED CYCLE FOR DRILLING (G80–G89) 173. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.1 Front Drilling Cycle (G83) / Side Drilling Cycle (G87) 176. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.2 Front Tapping Cycle (G84) / Side Tapping Cycle (G88) 179. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.3 Front Boring Cycle (G85) / Side Boring Cycle (G89) 181. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.4 Canned Cycle for Drilling Cancel (G80) 182. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.5 Precautions to be Taken by Operator 183. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4 CANNED GRINDING CYCLE (FOR GRINDING MACHINE) 184. . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4.1 Traverse Grinding Cycle (G71) 184. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4.2 Traverse Direct Fixed–dimension Grinding Cycle (G72) 185. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4.3 Oscillation Grinding Cycle (G73) 186. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4.4 Oscillation Direct Fixed–Dimension Grinding Cycle 187. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5 CHAMFERING AND CORNER R 188. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.6 MIRROR IMAGE FOR DOUBLE TURRET (G68, G69) 191. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.7 DIRECT DRA WING DIMENSIONS PROGRAMMING 192. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.8 RIGID TAPPING 197. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.8.1 Front Face Rigid Tapping Cycle (G84) / Side Face Rigid Tapping Cycle (G88) 198. . . . . . . . . . . . . . . . . . . .

15.COMPENsation FUNCTION 201. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1 TOOL OFFSET 202. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1.1 Tool Geometry Offset and Tool Wear Offset 202. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1.2 T Code for Tool Offset 203. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–3

T ABLE OF CONTENTS

15.1.3 Tool Selection 203. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1.4 Offset Number 203. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1.5 Offset 204. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1.6 G53, G28, G30, and G30.1 Commands When Tool Position Offset is Applied 207. . . . . . . . . . . . . . . . . . . . .

15.2 OVERVIEW OF TOOL NOSE RADIUS COMPENSATION 211. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.1 Imaginary Tool Nose 211. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.2 Direction of Imaginary Tool Nose 213. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.3 Offset Number and Offset Value 214. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.4 Work Position and Move Command 216. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.5 Notes on tool nose radius compensation 221. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3 DETAILS OF TOOL NOSE RADIUS COMPENSA TION 224. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3.1 General 224. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3.2 Tool Movement in Start–up 226. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3.3 Tool Movement in Offset Mode 228. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3.4 Tool Movement in Offset Mode Cancel 241. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3.5 Interference Check 244. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3.6 Overcutting by Tool Nose Radius Compensation 249. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3.7 Correction in Chamfering and Corner Arcs 250. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3.8 Input Command from MDI 252. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3.9 General Precautions for Offset Operations 253. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3.10 G53, G28, G30, and G30.1 Commands in Tool–tip Radius Compensation Mode 254. . . . . . . . . . . . . . . . . . .

15.4 CORNER CIRCULAR INTERPOLATION FUNCTION (G39) 263. . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.5 TOOL COMPENSATION VALUES, NUMBER OF COMPENSATION VALUES,

AND ENTERING VALUES FROM THE PROGRAM (G10) 265. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.5.1 Tool Compensation and Number of Tool Compensation 265. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.5.2 Changing of Tool Offset Value (Programmable Data Input ) (G10) 266. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6 AUTOMATIC TOOL OFFSET (G36, G37) 267. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.7 COORDINATE ROTATION (G68.1, G69.1) 270. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–62754EN/01

16.CUSTOM MACRO 274. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.1 VARIABLES 275. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.2 SYSTEM VARIABLES 279. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.3 ARITHMETIC AND LOGIC OPERATION 285. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.4 MACRO STATEMENTS AND NC STATEMENTS 289. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5 BRANCH AND REPETITION 290. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5.1 Unconditional Branch (GOTO Statement) 290. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5.2 Conditional Branch (IF Statement) 291. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5.3 Repetition (While Statement) 292. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6 MACRO CALL 295. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.1 Simple Call (G65) 296. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.2 Modal Call (G66) 300. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.3 Macro Call Using G Code 302. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.4 Macro Call Using an M Code 303. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.5 Subprogram Call Using an M Code 304. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.6 Subprogram Calls Using a T Code 305. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.7 Sample Program 306. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.7 PROCESSING MACRO STATEMENTS 308. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.8 REGISTERING CUSTOM MACRO PROGRAMS 310. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.9 LIMITATIONS 311. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–4

B–62754EN/01

16.10 EXTERNAL OUTPUT COMMANDS 312. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.11 INTERRUPTION TYPE CUST OM MACRO 316. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.11.1 Specification Method 317. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.11.2 Details of Functions 318. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

T ABLE OF CONTENTS

17.PROGRAMMABLE PARAMETER ENTRY (G10) 325. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.MEMORY OPERATION BY FS15 TAPE FORMAT 328. . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.1 ADDRESSES AND SPECIFIABLE VALUE RANGE FOR SERIES 15 TAPE FORMAT 329. . . . . . .

18.2 EQUAL–LEAD THREADING 330. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.3 SUBPROGRAM CALLING 331. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.4 CANNED CYCLE 332. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.5 MULTIPLE REPETITIVE CANNED TURNING CYCLE 333. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.6 CANNED DRILLING CYCLE FORMATS 335. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19.FUNCTIONS FOR HIGH SPEED CUTTING 339. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19.1 HIGH SPEED CYCLE CUTTING 340. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19.2 DISTRIBUTION PROCESSING TERMINATION MONITORING FUNCTION

FOR THE HIGH–SPEED MACHINING COMMAND (G05) 342. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.AXIS CONTROL FUNCTION 343. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.1 POLYGONAL TURNING 344. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.2 ROTARY AXIS ROLL–OVER 349. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.3 SIMPLE SYNCHRONIZATION CONTROL 350. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.4 SYNCHRONIZATION CONTROL 352. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.5 B–AXIS CONTROL (G100, G101, G102, G103, G110) 353. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.6 ANGULAR AXIS CONTROL / ARBITRARY ANGULAR AXIS CONTROL 363. . . . . . . . . . . . . . . .

20.7 TOOL WITHDRAWAL AND RETURN (G10.6) 365. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.TWO–PATH CONTROL FUNCTION 368. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.1 GENERAL 369. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.2 WAITING FOR TOOL POSTS 371. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.3 TOOL POST INTERFACE CHECK 373. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.3.1 General 373. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.3.2 Data Setting for the Tool Post Interference Check Function 373. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.3.3 Setting and Display of Interference Forbidden Areas for Tool Post Interference Checking 377. . . . . . . . . . . .

21.3.4 Conditions for Making a Tool Post Interference Check 378. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.3.5 Execution of Tool Post Interference Checking 379. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.3.6 Example of Making a Tool Post Interference Check 381. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.4 BALANCE CUT (G68, G69) 383. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.5 MEMOR Y COMMON TO TOOL POSTS 385. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.6 SPINDLE CONTROL IN TWO–PATH CONTROL 386. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21.7 SYNCHRONIZATION CONTROL AND COMPOSITE CONTROL 388. . . . . . . . . . . . . . . . . . . . . . . .

22.PATTERN DATA INPUT FUNCTION 391. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

22.1 DISPLAYING THE PATTERN MENU 392. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

22.2 PATTERN DATA DISPLAY 396. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

22.3 CHARACTERS AND CODES TO BE USED FOR THE PATTERN DATA

INPUT FUNCTION 400. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–5

T ABLE OF CONTENTS

B–62754EN/01

III. OPERATION

1. GENERAL 405. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.1 MANUAL OPERATION 406. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.2 TOOL MOVEMENT BY PROGRAMING – AUTOMATIC OPERATION 408. . . . . . . . . . . . . . . . . . .

1.3 AUTOMATIC OPERATION 409. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4 TESTING A PROGRAM 411. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4.1 Check by Running the Machine 411. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4.2 How to View the Position Display Change without Running the Machine 412. . . . . . . . . . . . . . . . . . . . . . . .

1.5 EDITING A PART PROGRAM 413. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.6 DISPLAYING AND SETTING DATA 414. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7 DISPLAY 417. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.1 Program Display 417. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.2 Current Position Display 418. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.3 Alarm Display 418. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.4 Parts Count Display, Run Time Display 419. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.5 Graphic Display (See Section III–12) 420. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.8 DATA OUTPUT 421. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2. OPERATIONAL DEVICES 422. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1 SETTING AND DISPLAY UNIT 423. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.1 9″ Monochrome CRT/MDI (Small Type) 424. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.2 9″ Monochrome CRT/MDI (Standard Type) 424. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.3 9″ Monochrome PDP/MDI (Standard Type) 425. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.4 8.4″ Color LCD/MDI (Small Type, Sheet Key) 426. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.5 8.4″ Color LCD/MDI (Standard Type, Sheet Key) 427. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.6 9.5″ Color LCD/MDI (Horizontal Type) 427. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.7 9.5″ Color LCD/MDI (Vertical Type) 428. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.8 14″ Color CRT/MDI (Horizontal Type) 429. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.9 14″ Color CRT/MDI (Vertical Type) 430. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.10 9″ Monochrome CRT (Separate Type) 431. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.11 9″ Monochrome PDP (Separate Type) 431. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.12 7.2″ Monochrome LCD (Separate type) 432. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.13 8.4″ Color LCD (Separate type) 432. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.14 9.5″ Color LCD (Separate Type) 433. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.15 Separate Type MDI (Small Key) for 9″CRT/PDP, 8.4″/7.2″LCD 434. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.16 Separate Type MDI (Standard Key) for 9″CRT/PDP, 8.4″/7.2″LCD 435. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.17 Separate Type MDI (Vertical Type) for 9.5″LCD 436. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.18 Separate Type MDI (Horizontal Type) for 9.5″LCD 437. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.2 EXPLANATION OF THE KEYBOARD 438. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3 FUNCTION KEYS AND SOFT KEYS 440. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.1 General Screen Operations 440. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.2 Function Keys 441. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.3 Soft Keys 442. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.4 Key Input and Input Buffer 458. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.5 Warning Messages 459. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.6 14″ CRT and 9.5″ LCD Soft Key Configuration 460. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4 EXTERNAL I/O DEVICES 461. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.1 FANUC Handy File 463. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–6

B–62754EN/01

2.4.2 FANUC Floppy Cassette 463. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.3 FANUC FA Card 464. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.4 FANUC PPR 464. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.5 Portable Tape Reader 465. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5 POWER ON/OFF 466. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.1 Turning on the Power 466. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.2 Screen Displayed at Power–on 467. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.3 Power Disconnection 468. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

T ABLE OF CONTENTS

3. MANUAL OPERATION 469. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.1 MANUAL REFERENCE POSITION RETURN 470. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.2 JOG FEED 472. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.3 INCREMENTAL FEED 474. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.4 MANUAL HANDLE FEED 475. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.5 MANUAL ABSOLUTE ON AND OFF 478. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.6 MANUAL LINEAR/CIRCULAR INTERPOLATION 483. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4. AUTOMATIC OPERATION 488. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.1 MEMOR Y OPERATION 489. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.2 MDI OPERATION 492. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.3 PROGRAM REST ART 496. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.4 SCHEDULING FUNCTION 504. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.5 SUBPROGRAM CALL FUNCTION (M198) 509. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.6 MANUAL HANDLE INTERRUPTION 511. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.7 MIRROR IMAGE 514. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8 MANUAL INTERVENTION AND RETURN 516. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.9 DNC OPERATION 518. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5. TEST OPERATION 521. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.1 MACHINE LOCK AND AUXILIAR Y FUNCTION LOCK 522. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.2 FEEDRATE OVERRIDE 524. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.3 RAPID TRAVERSE OVERRIDE 525. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4 DRY RUN 526. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.5 SINGLE BLOCK 527. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6. SAFETY FUNCTIONS 531. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.1 EMERGENCY STOP 532. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.2 OVERTRAVEL 533. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.3 STROKE CHECK 534. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.4 CHUCK AND TAILSTOCK BARRIERS 538. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.5 STROKE LIMIT CHECK PRIOR TO PERFORMING MOVEMENT 545. . . . . . . . . . . . . . . . . . . . . . .

7. ALARM AND SELF–DIAGNOSIS FUNCTIONS 548. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1 ALARM DISPLAY 549. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2 ALARM HISTORY DISPLAY 551. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.3 CHECKING BY SELF–DIAGNOSTIC SCREEN 552. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8. DATA INPUT/OUTPUT 555. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1 FILES 556. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–7

T ABLE OF CONTENTS

8.2 FILE SEARCH 558. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3 FILE DELETION 560. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4 PROGRAM INPUT/OUTPUT 561. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.1 Inputting a Program 561. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.2 Outputting a Program 564. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5 OFFSET DATA INPUT AND OUTPUT 566. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5.1 Inputting Offset Data 566. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5.2 Outputting Offset Data 567. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6 INPUTTING AND OUTPUTTING PARAMETERS AND

PITCH ERROR COMPENSATION DATA 568. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.1 Inputting Parameters 568. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.2 Outputting Parameters 569. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.3 Inputting Pitch Error Compensation Data 570. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.4 Outputting Pitch Error Compensation Data 571. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.7 INPUTTING / OUTPUTTING CUSTOM MACRO COMMON VARIABLES 572. . . . . . . . . . . . . . . .

8.7.1 Inputting Custom Macro Common Variables 572. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.7.2 Outputting Custom Macro Common Variable 573. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8 DISPLAYING DIRECTORY OF FLOPPY DISK 574. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.1 Displaying the Directory 575. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.2 Reading Files 578. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.3 Outputting Programs 579. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.4 Deleting Files 580. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.9 OUTPUTTING A PROGRAM LIST FOR A SPECIFIED GROUP 582. . . . . . . . . . . . . . . . . . . . . . . . .

B–62754EN/01

9. EDITING PROGRAMS 583. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1 INSERTING, ALTERING AND DELETING A WORD 584. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.1 Word Search 585. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.2 Heading a Program 587. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.3 Inserting a Word 588. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.4 Altering a Word 589. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.5 Deleting a Word 590. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2 DELETING BLOCKS 591. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.1 Deleting a Block 591. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.2 Deleting Multiple Blocks 592. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3 PROGRAM NUMBER SEARCH 593. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4 SEQUENCE NUMBER SEARCH 594. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5 DELETING PROGRAMS 596. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.1 Deleting One Program 596. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.2 Deleting All Programs 596. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.3 Deleting More Than One Program by Specifying a Range 597. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6 EXTENDED PART PROGRAM EDITING FUNCTION 598. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.1 Copying an Entire Program 599. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.2 Copying Part of a Program 600. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.3 Moving Part of a Program 601. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.4 Merging a Program 602. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.5 Supplementary Explanation for Copying, Moving and Merging 603. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.6 Replacement of Words and Addresses 605. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.7 EDITING OF CUSTOM MACROS 607. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.8 BACKGROUND EDITING 608. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.9 PASSWORD FUNCTION 609. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–8

B–62754EN/01

T ABLE OF CONTENTS

10.CREATING PROGRAMS 611. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.1 CREATING PROGRAMS USING THE MDI PANEL 612. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2 AUTOMATIC INSERTION OF SEQUENCE NUMBERS 613. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.3 CREATING PROGRAMS IN TEACH IN MODE 615. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.4 CONVERSATIONAL PROGRAMMING WITH GRAPHIC FUNCTION 618. . . . . . . . . . . . . . . . . . . .

11.SETTING AND DISPLAYING DATA 622. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1 SCREENS DISPLAYED BY FUNCTION KEY

POS

11.1.1 Position Display in the Workpiece Coordinate System 631. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.2 Position Display in the Relative Coordinate System 633. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.3 Overall Position Display 636. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.4 Presetting the Workpiece Coordinate System 638. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.5 Actual Feedrate Display 639. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.6 Display of Run Time and Parts Count 641. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.7 Setting the Floating Reference Position 642. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.8 Operating Monitor Display 643. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2 SCREENS DISPLAYED BY FUNCTION KEY

PROG

(IN MEMORY MODE OR MDI MODE) 645. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.1 Program Contents Display 646. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.2 Current Block Display Screen 647. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.3 Next Block Display Screen 648. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.4 Program Check Screen 649. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.5 Program Screen for MDI Operation 652. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.6 Stamping the Machining Time 653. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.7 Displaying the B–axis Operation State 661. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3 SCREENS DISPLAYED BY FUNCTION KEY

11.3.1 Displaying Memory Used and a List of Programs 663. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3.2 Two–path simultaneous editing on the program screen 666. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3.3 Displaying a Program List for a Specified Group 669. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4 SCREENS DISPLAYED BY FUNCTION KEY

PROG

(IN THE EDIT MODE) 662. . . . . . . . . . . . . . .

OFFSET SETTING

630. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

672. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.1 Setting and Displaying the Tool Offset Value 673. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.2 Direct Input of Tool Offset Value 676. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.3 Direct Input of tool offset measured B 678. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.4 Counter Input of Offset value 680. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.5 Setting the Workpiece Coordinate System Shifting Amount 681. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.6 Y Axis Offset 683. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.7 Displaying and Entering Setting Data 686. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.8 Sequence Number Comparison and Stop 688. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.9 Displaying and Setting Run Time,Parts Count, and Time 690. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.10 Displaying and Setting the Workpiece Origin Offset Value 692. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.11 Input of measured workpiece origin offsets 693. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.12 Displaying and Setting Custom Macro Common Variables 695. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.13 Displaying and Setting the Software Operator’s Panel 696. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.14 Displaying and Setting Tool Life Management Data 698. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.15 Setting and Displaying B–axis Tool Compensation 701. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5 SCREENS DISPLAYED BY FUNCTION KEY

SYSTEM

c–9

703. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

T ABLE OF CONTENTS

11.5.1 Displaying and Setting Parameters 704. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5.2 Displaying and Setting Pitch Error Compensation Data 706. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

AND WARNING MESSAGES FOR DATA SETTING OR INPUT/OUTPUT OPERATION 708. . . . .

11.6.1 Displaying the Program Number and Sequence Number 708. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.6.2 Displaying the Status and Warning for Data Setting or Input/Output Operation 709. . . . . . . . . . . . . . . . . . . .

B–62754EN/01

11.7 SCREENS DISPLAYED BY FUNCTION KEY

11.7.1 External Operator Message History Display 711. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8 CLEARING THE SCREEN 713. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8.1 Erase CRT Screen Display 713. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8.2 Automatic Erase CRT Screen Display 714. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

MESSAGE

12.GRAPHICS FUNCTION 715. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.1 GRAPHICS DISPLAY 716. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.HELP FUNCTION 722. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

IV. MAINTENANCE

1. METHOD OF REPLACING BATTERY 729. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.1 REPLACING CNC BATTERY FOR MEMORY BACK–UP 730. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.2 REPLACING BATTERIES FOR ABSOLUTE PULSE CODER 731. . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.3 REPLACING BATTERIES FOR ABSOLUTE PULSE CODER

( Series Servo Amp Module) 732. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

711. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

APPENDIX

A. TAPE CODE LIST 735. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B. LIST OF FUNCTIONS AND TAPE FORMAT 737. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

C. RANGE OF COMMAND VALUE 740. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D. NOMOGRAPHS 743. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D.1 INCORRECT THREADED LENGTH 744. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D.2 SIMPLE CALCULATION OF INCORRECT THREAD LENGTH 746. . . . . . . . . . . . . . . . . . . . . . . . .

D.3 TOOL PATH AT CORNER 748. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D.4 RADIUS DIRECTION ERROR AT CIRCLE CUTTING 751. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

E. STATUS WHEN TURNING POWER ON, WHEN CLEAR AND WHEN RESET 752. . . .

F. CHARACTER–TO–CODES CORRESPONDENCE TABLE 754. . . . . . . . . . . . . . . . . . . . .

G. ALARM LIST 755. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

H. OPERATION OF PORTABLE TAPE READER 776. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–10

I. GENERAL

B–62754EN/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 (Table1).

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–TC 16–TC Series 16

FANUC Series 18–TC 18–TC Series 18

FANUC Series 160–TC 160–TC Series 160

FANUC Series 180–TC 180–TC Series 180

1. GENERAL

GENERAL

B–62754EN/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–62754EN/01

Cutting 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 cutting process

4. Cutting tools and cutting conditions

Decide the cutting method in every cutting process.

Cutting procedure

1. Cutting method : Rough Semi Finish

2. Cutting tools

3. Cutting conditions : Feedrate Cutting depth

4. Tool path

1 2 3

End face

cutting

Outer diameter

cutting

Grooving

1. GENERAL

GENERAL

B–62754EN/01

Grooving

Outer diameter cutting

Workpiece

End face cutting

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

B–62754EN/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–62754EN/01



PROGRAMMING

1. GENERAL

PROGRAMMING

B–62754EN/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).

Tool

Workpiece

Fig.1.1 (a) T ool movement along the straight line which is parallel to Z–axis

Program G01 Z...;

D Tool movement along an

arc

Tool

Workpiece

Fig.1.1 (b) T ool movement along the taper line

Workpiece

Tool

Program G02X ... Z ... R ... ; or G03X ... Z ... R ... ;

Program G01 X ... Z... ;

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

B–62754EN/01

PROGRAMMING

1. GENERAL

The term interpolation refers to an operation in which the tool moves along a straight line or arc in the way described above. 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 Z__; X––Z––––;

Control unit

Interpolation

a) Movement

along straight line

b) Movement

along arc

Fig. 1.1 (d) Interpolation function

(b) Movement along arc

G03X––Z––;

X axis

Y axis

Tool movement

NOTE

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

D Thread cutting

Threads can be cut by moving the tool in synchronization with spindle rotation. In a program, specify the thread cutting function by G32.

Workpiece

Fig. 1.1 (e) Straight thread cutting

Tool

Program G32Z––F––;

1. GENERAL

PROGRAMMING

B–62754EN/01

Workpiece

Tool

Program G32X––Z––F––;

Fig. 1.1 (f) Taper thread cutting

B–62754EN/01

PROGRAMMING

1. GENERAL

1.2

FEED– FEED FUNCTION

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

Chuck

Workpiece

Fig. 1.2 (a) Feed function

Tool

Feedrates can be specified by using actual numerics. For example, the following command can be used to feed the tool 2 mm while the workpiece makes one turn :

F2.0

The function of deciding the feed rate is called the feed function (See II–5).

1. GENERAL

1.3

PART DRAWING AND TOOL MOVEMENT

PROGRAMMING

B–62754EN/01

1.3.1

Reference Position (Machine–Specific Position)

Explanations

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.

Tool post

Chuck

Fig. 1.3.1 (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.

Reference position

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.

B–62754EN/01

1.3.2

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

PROGRAMMING

Part drawing

1. GENERAL

Program

Coordinate system

CNC

Command

Workpiece

Explanations

D Coordinate system

Machine tool

Fig. 1.3.2 (a) 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. 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

1. GENERAL

PROGRAMMING

B–62754EN/01

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.

D Methods of setting the

two coordinate systems in the same position

The following method is usually used to define two coordinate systems at the same location.

1. When coordinate zero point is set at chuck face

Workpiece

150

Fig. 1.3.2 (c) Coordinates and dimensions on part drawing

Workpiece

Fig. 1.3.2 (d) Coordinate system on lathe as specified by CNC (made to coincide with the coordinate system on part drawing)

B–62754EN/01

PROGRAMMING

2. When coordinate zero point is set at work end face.

1. GENERAL

Workpiece

100

Fig. 1.3.2 (e) Coordinates and dimensions on part drawing

Workpiece

Fig. 1.3.2 (f) Coordinate system on lathe as specified by CNC

(made to coincide with the coordinate system on part drawing)

1. GENERAL

1.3.3

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

PROGRAMMING

B–62754EN/01

Explanations

D Absolute command

Methods of command for moving the tool can be indicated by absolute or incremental designation (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.

Tool

Workpiece

φ30

Command specifying movement from point A to point B

G90X30.0Z70.0;

110

Fig. 1.3.3 (a) Absolute command

Coordinates of point B

B–62754EN/01

PROGRAMMING

1. GENERAL

D Incremental command

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

Tool

φ60

φ30

Command specifying movement from point A to point B

U–30.0W–40.0

Distance and direction for movement along each axis

D Diameter programming /

radius programming

Fig. 1.3.3 (b) Incremental command

Dimensions of the X axis can be set in diameter or in radius. Diameter programming or radius programming is employed independently in each machine.

1. Diameter programming

In diameter programming, specify the diameter value indicated on the drawing as the value of the X axis.

φ30

Workpiece

φ40

Coordinate values of points A and B

A(30.0, 80.0), B(40.0, 60.0)

Fig. 1.3.3 (c) Diameter programming

1. GENERAL

PROGRAMMING

B–62754EN/01

2. Radius programming

In radius programming, specify the distance from the center of the workpiece, i.e. the radius value as the value of the X axis.

Workpiece

Coordinate values of points A and B

A(15.0, 80.0), B(20.0, 60.0)

Fig. 1.3.3 (d) Radius programming

B–62754EN/01

PROGRAMMING

1. GENERAL

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

Workpiece

Fig. 1.4 (a) Cutting speed

V: Cutting speed

v m/min

φ

N rpm

The spindle speed is approximately 478 rpm, which is obtained from N=1000v/πD. Hence the following command is required:

S478 ;

Commands related to the spindle speed are called the spindle speed function (See II–10). The cutting speed v (m/min) can also be specified directly by the speed value. Even when the workpiece diameter is changed, the CNC changes the spindle speed so that the cutting speed remains constant. This function is called the constant surface speed control function (See II–10.2).

1. GENERAL

PROGRAMMING

B–62754EN/01

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

Fig. 1.5 (a) T ool used for various machining

Tool post

When the tool is stored at location 01 of the tool post, the tool can be selected by specifying T0101. This is called the tool function (See II–11).

B–62754EN/01

PROGRAMMING

1. GENERAL

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 (See II–12).

Coolant on/off

Chuck open/close

Workpiece

Fig. 1.6 (a) Command for machine operations

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. For example, when M03 is specified, the spindle is rotated clockwise at the specified spindle speed.

CW spindle rotation

1. GENERAL

PROGRAMMING

B–62754EN/01

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

Block

⋅ ⋅ ⋅ ⋅

Block

Fig. 1.7 (a) Program configuration

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).

B–62754EN/01

PROGRAMMING

1. GENERAL

Explanations

D Block

D Program

The block and the program have the following configurations.

1 block

N fffff G ff Xff.f Zfff.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 begins with a sequence number that identifies that 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.

1. GENERAL

PROGRAMMING

B–62754EN/01

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

B–62754EN/01

1.8

TOOL FIGURE AND TOOL MOTION BY PROGRAM

Explanations

PROGRAMMING

1. GENERAL

D Machining using the end

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

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.

Workpiece

Standard tool

Rough cutting tool

Fig. 1.8 (a) T ool offset

Finishing tool

Grooving tool

Thread cutting tool

1. GENERAL

PROGRAMMING

B–62754EN/01

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. Besides the stroke limits, data in memory can be used to define an area which tools cannot enter.

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 (see Section III–11). This function is called stroke check.

B–62754EN/01

PROGRAMMING

CONTROLLED AXES

2. CONTROLLED AXES

2.1

CONTROLLED AXES

Series 16 Series 160

PROGRAMMING

Item

Number of basic controlled axes

Controlled axis expansion (total)

Number of basic simultaneously controlled axes

Simultaneously controlled axis expansion (total)

16–TC

160–TC

2 axes 2 axes for each tool post

Max. 8 axes (Included in Cs axis)

2 axes 2 axes for each tool post

Max. 6 axes Max. 4 axes for each tool

(two–path control)

(4 axes in total) Max. 6 axes for each tool

post +Cs axis (Note)

(4 axes in total)

post

B–62754EN/01

16–TC, 160–TC

NOTE

1 A two–path control system with a 9–inch CRT has up to

eight controlled axes.

2 The number of simultaneously controllable axes for manual

operation (jog feed, incremental feed, or manual handle feed) is 1 or 3 (1 when bit 0 (JAX) of parameter 1002 is set to 0 and 3 when it is set to 1).

Series 18 Series 180

Item

Number of basic controlled axes

Controlled axis expansion (total)

Number of basic simultaneously controlled axes

Simultaneously controlled axis expansion (total)

18–TC

180–TC

2 axes 2 axes for each tool post

Max. 6 axes (Included in Cs axis)

2 axes 2 axes for each tool post

Max. 4 axes Max. 4 axes for each tool

18–TC, 180–TC

(two–path control)

(4 axes in total) Max. 4 axes for each tool

post +Cs axis (Note)

(4 axes in total)

post

NOTE

1 A two–path control system with a 9–inch CRT has up to

eight controlled axes.

2 The number of simultaneously controllable axes for manual

operation (jog feed, incremental feed, or manual handle feed) is 1 or 3 (1 when bit 0 (JAX) of parameter 1002 is set to 0 and 3 when it is set to 1).

B–62754EN/01

PROGRAMMING

2. CONTROLLED AXES

2.2

NAMES OF AXES

Limitations

D Default axis name

D Duplicate axis name

The names of two basic axes are always X and Z; the names of additional axes can be optionally selected from A, B, C, U, V, W, and Y by using parameter No.1020. Each axis name is determined according to parameter No. 1020. If the parameter specifies 0 or anything other than the nine letters, the axis name defaults to a number from 1 to 8. With two–path control, the names of two basic axes for one tool post are always X and Z; the names of additional axes can be optionally selected from A, B, C, U, V, W, and Y by using parameter No. 1020. For one tool post, the same axis name cannot be assigned to multiple axes, but the same axis name can be used with the other tool post.

When a default axis name (1 to 8) is used, the system cannot operate in MEM or MDI mode.

If the parameter specifies an axis name more than once, only the first axis to be assigned that axis name becomes operable.

NOTE

1 When G code system A is used, the letters U, V, and W

cannot be used as an axis name (hence, the maximum of six controlled axes), because these letters are used as incremental commands for X, Y, and Z. To use the letters U, V, and W as axis names, the G code system must be B or C. Likewise, letter H is used as an incremental command for C, thus incremental commands cannot be used if A or B is used as an axis name.

2 With two–path control, when information (such as the

current position) about each axis is displayed on the CRT screen, an axis name may be followed by a subscript to indicate a tool post number (e.g.,X1 and X2). This is axis name to help the user to easily understand which tool post an axis belongs to. When writing a program, the user must specify X, Y, Z, U, V, W, A, B, and C without attaching a subscript.

3 In G76 (multiple–thread cutting), the A address in a block

specifies the tool nose angle instead of a command for axis A. If C or A is used as an axis name, C or A cannot be used as an angle command for a straight line in chamfering or direct drawing dimension programming. Therefore, C and A should be used according to bit 4 (CCR) of parameter No.

3405.

2. CONTROLLED AXES

ce i

PROGRAMMING

B–62754EN/01

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 degrees. The increment system is classified into IS–B and IS–C (T ables 2.3(a) and

2.3(b)). Select IS–B or IS–C using bit 1 (ISC) of parameter 1004. When

the IS–C increment system is selected, it is applied to all axes and the 1/10 increment system option is required.

T able 2.3 (a) Increment system IS–B

Least input increment Least command increment

Metric system machine

Inch machine system

npu

inch

npu

inch

npu

0.001mm(Diameter) 0.0005mm

0.001mm(Radius) 0.001mm

0.001deg 0.001deg

0.0001inch(Diameter) 0.0005mm

0.0001inch(Radius) 0.001mm

0.001deg 0.001deg

0.001mm(Diameter) 0.00005inch

0.001mm(Radius) 0.0001inch

0.001deg 0.001deg

0.0001inch(Diameter) 0.00005inch

0.0001inch(Radius) 0.0001inch

0.001deg 0.001deg

Metric system machine

Inch machine system

T able 2.3 (b) Increment system IS–C

Least input increment Least command increment

npu

inch

npu

inch

npu

0.0001mm(Diameter) 0.00005mm

0.0001mm(Radius) 0.0001mm

0.0001deg 0.0001deg

0.00001inch(Diameter) 0.00005mm

0.00001inch(Radius) 0.0001mm

0.0001deg 0.0001deg

0.0001mm(Diameter) 0.000005inch

0.0001mm(Radius) 0.00001inch

0.0001deg 0.0001deg

0.00001inch(Diameter) 0.000005inch

0.00001inch(Radius) 0.00001inch

0.0001deg 0.0001deg

B–62754EN/01

IS–B

IS–C

PROGRAMMING

2. CONTROLLED AXES

2.4

MAXIMUM STROKES

The maximum stroke controlled by this CNC is shown in the table below: Maximum stroke=Least command increment99999999

T able 2.4 (a) Maximum strokes

Increment system

Metric machine system

–

Inch machine system

Metric machine system

–

Inch machine system

Maximum strokes

99999.999 mm 99999.999 deg

9999.9999 inch 99999.999 deg

9999.9999 mm 9999.9999 deg

999.99999 inch 9999.9999 deg

NOTE

1 The unit in the table is a diameter value with diameter

programming and a radius value in radius programming.

2 A command exceeding the maximum stroke cannot be

specified.

3 The actual stroke depends on the machine tool.

3. PREPARATORY FUNCTION (G FUNCTION)

PREPARATORY FUNCTION (G FUNCTION )

PROGRAMMING

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.

B–62754EN/01

G01X_;

Z_;

X_;

G00Z_;

There are three G code systems : A,B, and C (Table 3). Select a G code system using bits 6 (GSB) and 7 (GSC) of parameter 3401. Generally , this manual describes the use of G code system A, except when the described item can use only G code system B or C. ln such cases, the use of G code system B or C is described.

G01 is effective in this range

B–62754EN/01

PROGRAMMING

3. PREP ARATORY FUNCTION (G FUNCTION)

Explanations

1. If the CNC enters the clear state (see bit 6 (CLR) of parameter 3402) when the power is turned on or the CNC is reset, the modal G codes change as follows.

(1)G codes marked with

in Table 3 are enabled.

(2)When the system is cleared due to power–on or reset, whichever

specified, either G20 or G21, remains effective.

(3)Bit 7 of parameter No. 3402 can be used to specify whether G22

or G23 is selected upon power–on. Resetting the CNC to the clear state does not affect the selection of G22 or G23.

(4) Setting bit 0 (G01) of parameter 3402 determines which code,

either G00 or G01, is effective.

(5) Setting bit 3 (G91) of parameter 3402 determines which code,

either G90 or G91, is effective.

2. G codes of group 00 except G10 and G11 are single–shot G codes.

3. P/S larm (No.010) is displayed when a G code not listed in the G code list is specified or a G code without a corresponding option is specified.

4. G codes of different groups can be specified in the same block. If G codes of the same group are specified in the same block, the G code specified last is valid.

5. If a G code of group 01 is specified in a canned cycle, the canned cycle is canceled in the same way as when a G80 command is specified. G codes of group 01 are not affected by G codes for specifying a canned cycle.

6. When G code system A is used for a canned cycle, only the initial level is provided at the return point.

7. G codes are displayed for each group number.

3. PREPARATORY FUNCTION

Grou

Function

(G FUNCTION)

G code

A B C

G00 G00 G00 G01 G01 G01

G02 G02 G02 G03 G03 G03 Circular interpolation CCW or Helical interpolation CCW G04 G04 G04 Dwell G05 G05 G05 High speed cycle cutting

G07.1

(G107)

G10

G10.6 G10.6 G10.6 Tool retract & recover

G11 G11 G11 Programmable data input cancel

G12.1

(G112)

G13.1

(G113)

G17 G17 G17 G18 G18 G18

G19 G19 G19 Y pZp plane selection G20 G20 G70 G21 G21 G71 G22 G22 G22 G23 G23 G23 G25 G25 G25 G26 G26 G26 G27 G27 G27 Reference position return check G28 G28 G28 Return to reference position G30 G30 G30 00 2nd, 3rd and 4th reference position return

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

G31 G31 G31 Skip function G32 G33 G33 G34 G34 G34 G36 G36 G36 Automatic tool compensation X G37 G37 G37 00 Automatic tool compensation Z G39 G39 G39 Corner circular interpolation G40 G40 G40 G41 G41 G41 G42 G42 G42 Tool nose radius compensation right G50 G92 G92

G50.3 G92.1 G92.1

G07.1

(G107)

G10 G10

G12.1

(G112)

G13.1

(G113)

G07.1

(G107)

G12.1

(G112)

G13.1

(G113)

PROGRAMMING

Table 3 G code list (1/3)

B–62754EN/01

Positioning (Rapid traverse) Linear interpolation (Cutting feed) Circular interpolation CW or Helical interpolation CW

Cylindrical interpolation Programmable data input

Polar coordinate interpolation mode

Polar coordinate interpolation cancel mode XpY p plane selection

ZpXp plane selection

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

Thread cutting V ariable–lead thread cutting

Tool nose radius compensation cancel Tool nose radius compensation left

Coordinate system setting or max. spindle speed setting Workpiece coordinate system preset

B–62754EN/01

Grou

Function

20 00

A B C

G50.2

(G250)

G51.2

(G251)

G52 G52 G52 G53 G53 G53 G54 G54 G54 G55 G55 G55 G56 G56 G56 G57 G57 G57 G58 G58 G58 Workpiece coordinate system 5 selection G59 G59 G59 Workpiece coordinate system 6 selection G65 G65 G65 00 Macro calling G66 G66 G66 G67 G67 G67 G68 G68 G68 G69 G69 G69

G70 G70 G72 Finishing cycle G71 G71 G73 G72 G72 G74 G73 G73 G75 Pattern repeating G74 G74 G76 End face peck drilling G75 G75 G77 Outer diameter/internal diameter drilling G76 G76 G78 Multiple threading cycle G71 G71 G72 Traverse grinding cycle (for grinding machine)

G72 G72 G73 G73 G73 G74 Oscilation grinding cycle (for grinding machine) G74 G74 G75 G80 G80 G80

G83 G83 G83 Cycle for face drilling G84 G84 G84 G86 G86 G86 G87 G87 G87 Cycle for side drilling G88 G88 G88 Cycle for side tapping G89 G89 G89 Cycle for side boring G90 G77 G20 Outer diameter/internal diameter cutting cycle G92 G78 G21 01 Thread cutting cycle G94 G79 G24 Endface turning cycle G96 G96 G96 G97 G97 G97

G code

G50.2

(G250)

G51.2

(G251)

G50.2

(G250)

G51.2

(G251)

PROGRAMMING

Table 3 G code list (2/3)

Polygonal turning cancel

Polygonal turning Local coordinate system setting

Machine coordinate system setting Workpiece coordinate system 1 selection Workpiece coordinate system 2 selection

Workpiece coordinate system 3 selection Workpiece coordinate system 4 selection

Macro modal call Macro modal call cancel Mirror image for double turrets ON or balance cut mode

Mirror image for double turrets OFF or balance cut mode cancel

Stock removal in turning Stock removal in facing

Traverse direct constant–dimension grinding cycle (for grinding machine)

Oscilation direct constant–dimension grinding cycle (for grinding machine)

Canned cycle for drilling cancel

Cycle for face tapping Cycle for face boring

Constant surface speed control Constant surface speed control cancel

3. PREP ARATORY FUNCTION (G FUNCTION)

3. PREPARATORY FUNCTION

Grou

Function

(G FUNCTION)

G code

A B C

G98 G94 G94 G99



 G91 G91  G98 G98  G99 G99

G95 G95 G90 G90

PROGRAMMING

Table 3 G code list (3/3)

Per minute feed Per revolution feed Absolute programming Incremental programming Return to initial level (See Explanations 6) Return to R point level (See Explanations 6)

B–62754EN/01

PROGRAMMING

INTERPOLATION FUNCTIONS

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62754EN/01

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_;

_: For an absolute command, the coordinates of an end

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

Either of the following tool paths can be selected according to bit 1 (LRP) of parameter 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.

Linear interpolation positioning

End position

Non linear interpolation positioning

Start position

The rapid traverse rate in the G00 command is set to the parameter No.1420 for each axis independently by the machine tool builder. In the positioning 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.

B–62754EN/01

Examples

PROGRAMMING

56.0

4. INTERPOLA TION FUNCTIONS

30.5

30.0

Restrictions

φ40.0

< Radius programming >

G00X40.0Z56.0 ; (Absolute command)

G00U–60.0W–30.5;(Incremental command)

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

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62754EN/01

4.2

LINEAR INTERPOLATION (G01)

Format

Explanations

Tools can move along a line.

G01 _F_;

_: For an absolute command, the coordinates of an end

point , and for an incremental command, 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. For feed–per–minute mode under 2–axis simultaneous control, the feedrate for a movement along each axis as follows :

Examples

D Linear interpolation

G01ααββ

< Diameter programming >

G01X40.0Z20.1F20 ; (Absolute command) or G01U20.0W–25.9F20 ; (Incremental command)

Ff ;

Feed rate of α axis direction :

Feed rate of β axis direction :

L + 

) 2) 2) 

20.1

F +



46.0





φ40.0

End point

Start point

φ20.0

B–62754EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.3

CIRCULAR INTERPOLATION (G02, G03)

Format

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

Arc in the XpYp plane

G17

G02 G03

Arc in the ZpXp plane

G18

Arc in the YpZp plane

G19

G02 G03

Xp_Yp_

Xp_Zp_

Yp_Zp_

I_J_ R_

I_K_ R_

J_K_

Table.4.3 Description of the Command Format

Command Description

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 with

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

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)

sign, radius value

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

sign, radius value R_ Arc radius with no sign (always with radius value) F_ Feedrate along the arc

4. INTERPOLA TION FUNCTIONS

Explanations

PROGRAMMING

B–62754EN/01

NOTE

The U–, V–, and W–axes (parallel with the basic axis) can be used with G–codes B and C.

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 X (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,

pYp

plane

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

G02

G17

G03

G02

G18

G02

G19

G03

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.

D Full–circle programming

End point (x,y)

Center

Start point

End point (z,x)

Center

Start point

End point (y ,z)

Center

Start point

I0,J0, and K0 can be omitted. If the difference between the radius at the start point and that at the end point exceeds the value in a parameter (No.3410), an P/S alarm (No.020) occurs.

When X

p, Yp

, and Z

are omitted (the end point is the same as the start

point) and the center is specified with I, J, and K, a 360° arc (circle) is specified.

B–62754EN/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 considered. An arc with a sector angle of 180

°, and the other is more than 180° are

°or wider cannot be

specified. 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°)

G02 W60.0 U10.0 R50.0

For arc (2) (greater than 180°)

An arc with a sector angle of 180°

or wider cannot be specified within a single block.

F300.0 ;

(2)

Start point

r=50mm

End point

(1)

r=50mm

D Feedrate

Restrictions

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

tool nose radius 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, when a ZX plane is specified in G–code B or C, specifying the X–axis or U–axis (parallel to the X–axis) causes P/S alarm No. 028 to be generated. If the difference in the radius between the start and end points of the arc exceeds the value specified in parameter No. 3410, P/S alarm No. 020 is generated. If the end point is not on the arc, the tool moves in a straight line along one of the axes after reaching the end point. If an arc having a central angle approaching 180 is specified with R, the calculation of the center coordinates may produce an error. In such a case, specify the center of the arc with I, J, and K.

4. INTERPOLA TION FUNCTIONS

Examples

D Command of circular

interpolation X, Z

PROGRAMMING

B–62754EN/01

G02X_Z_I_K_F_; G03X_Z_I_K_F_;

End point

X–axis

Center of arc

(Absolute programming)

(Diameter programming)

Start point

Z–axis Z–axis Z–axis

End point

X–axis X–axis

(Absolute programming)

15.0

R25.0

10.0

φ50.0

30.0

G02X_Z_R_F_;

End point

(Diameter programming)

Start point

(Absolute programming)

(Diameter programming)

G02X50.0Z30.0I25.0F0.3; or G02U20.0W–020.0I25.0F0.3; or G02X50.0Z30.0R25.0F0.3 or G02U20.0W–20.0R25.F0.3;

Center of arc

(Diameter programming)

Start point

50.0

B–62754EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.4

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

R

JK R

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

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

Limitations

D Cutter compensation is applied only for a circular arc. D T ool offset and tool length compensation cannot be used in a block in

which a helical interpolation is commanded.

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62754EN/01

4.5

POLAR COORDINA TE INTERPOLA TION (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 method is useful in cutting a front surface and grinding a cam shaft on a lathe.

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)

G112 and G113 can be used in place of G12.1 and G13.1, respectively.

G12.1 starts the polar coordinate interpolation mode and selects a polar coordinate interpolation plane (Fig. 4.5 (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 workpiece coordinate system

Fig4.5 (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–62754EN/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

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 G04 G40, G41, G42

Circular interpolation.........

Dwell.............

Tool nose radius compensation . . . .

(Polar coordinate interpolation is applied to the path after cutter compensation.)

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

G98, G99

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).

D I and J in the Xp–Y p plane when the linear axis is the X–axis or an axis

parallel to the X–axis.

D J and K in the Yp–Zp plane when the linear axis is Y–axis or an axis

parallel to the Y–axis.

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

parallel to the Z–axis.

D Movement along axes

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

D Current position display

in the polar coordinate interpolation mode

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

NOTE

The U–, V–, and W–axes (parallel with the basic axis) can be used with G–codes B and C.

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

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).

4. INTERPOLA TION FUNCTIONS

Restrictions

PROGRAMMING

B–62754EN/01

Coordinate system for the polar coordinate interpolation

D Tool nose radius

 

D Program restart D Cutting feedrate for the

rotation axis

Before G12.1 is specified, a 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 nose radius compensation mode (G41 or G42). G12.1 or G13.1 must be specified in the tool nose radius compensation canceled mode (G40).

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 tool nose radius compensation is applied) does not move close to the center of the workpiece.

WARNING

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

∆

θ2

θ1

θ3

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.

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.

F < L × R ×

180

(mm/min)

D Diameter and radius

programming

Even when diameter programming is used for the linear axis (X–axis), radius programming is applied to the rotary axis (C–axis).

B–62754EN/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

N208

N207

Path after tool nose radius compensation

Program path

N201

N200

X axis

Tool

Z axis

X axis is by diameter programming, C axis is by radius programming.

O0001 ;

N010 T0101

N0100 G00 X120.0 C0 Z _ ; Positioning to start position N0200 G12.1 ; Start of polar coordinate interpolation N0201 G42 G01 X40.0 F _ ; N0202 C10.0 ; N0203 G03 X20.0 C20.0 R10.0 ; N0204 G01 X–40.0 ; Geometry program N0205 C–10.0 ; (program based on cartesian coordinates on N0206 G03 X–20.0 C–20.0 I10.0 J0 ; X–C’ plane) N0207 G01 X40.0 ; N0208 C0 ; N0209 G40 X120.0 ; N0210 G13.1 ; Cancellation of polar coordinate interpolation N0300 Z __ ; N0400 X __C __ ;

N0900M30 ;

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62754EN/01

4.6

CYLINDRICAL INTERPOLATION (G07.1)

Format

Explanations

D Plane selection

(G17, G18, G19)

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  r ; Starts the cylindrical interpolation mode

(enables cylindrical interpolation).

: : :

G07.1  0 ; The cylindrical interpolation mode is cancelled.

 : An address for the rotation axis

r : The radius of the cylinder

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

Use parameter No. 1002 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.

D Feedrate

NOTE

The U–, V–, and W–axes (parallel with the basic axis) can be used with G–codes B and C.

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

B–62754EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

D Circular interpolation

(G02,G03)

D Cutter compensation

D Cylindrical interpolation

accuracy

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 Section 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__;

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

Restrictions

D Arc radius specification

in the cylindrical interpolation mode

D Circular interpolation

and tool nose radius compensation

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

:Rounded to the least input increment

Specified value

2×2πR

MOTION REV

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 tool nose radius compensation is already applied, circular interpolation is not correctly performed in the cylindrical interpolation mode.

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62754EN/01

D Positioning

D Coordinate system

setting

D Cylindrical interpolation

mode setting

D Canned cycle for drilling

during cylindrical interpolation mode

Examples

In the cylindrical interpolation mode, positioning operations (including those that produce rapid traverse cycles such as G28, 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 G50 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.

Canned cycles for drilling, G81 to G89, cannot be specified during cylindrical interpolation mode.

Example of a Cylindrical Interpolation Program

O0001 (CYLINDRICAL INTERPOLATION ); N01 G00 Z100.0 C0 ; N02 G01 G18 W0 H0 ; N03 G07.1 H57299 ; N04 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 ; N1 1 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

90 70

N0 5

N06

N1 1

N07

N08

60 70

N09

N10

150

N12

230190

270

N13

360

deg

B–62754EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.7

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 enable. 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 them 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–62754EN/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–20.0 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–62754EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.8

CONSTANT LEAD THREADING (G32)

Fig. 4.8 (a) Straight Thread

Format

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

Fig. 4.8 (b) T apered Screw

Fig. 4.8 (c) Scroll Thread

G32_F_;

_: End point F_: Lead of the long axis

(always radius programming)

Explanations

X axis

End point

Fig. 4.8 (d) Example of Thread Cutting

Start point

Z axis

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.

4. INTERPOLA TION FUNCTIONS

mm in ut

0.0001 to 500.0000mm

Inch in ut

0.000001 inch to 9.999999inch

PROGRAMMING

Tapered thread

αx45° lead is LZ αy45° lead is LX

Fig. 4.8 (e) LZ and LX of a Tapered Thread

B–62754EN/01

In general, the lag of the servo system, etc. will produce somewhat incorrect leads at the starting and ending points of a thread cut. To compensate for this, a threading length somewhat longer than required should be specified. Table 4.8 (a) lists the ranges for specifying the thread lead.

T able. 4.8 (a) Ranges of lead sizes that can be specified

Least command increment

B–62754EN/01

Explanations

1. Straight thread cutting

X axis

PROGRAMMING

30mm

4. INTERPOLA TION FUNCTIONS

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

=3mm

δ2=1.5mm

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

2. T apered thread cutting

X axis

φ50

φ43

G00 U–62.0 ; G32 W–74.5 F4.0 ;

Z axis

G00 U62.0 ;

W74.5 ; U–64.0 ;

(For the second cut, cut 1mm more) G32 W–74.5 ; G00 U64.0 ;

W74.5 ;

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

=2mm

δ2=1mm

Cutting depth in the X axis direction is 1mm (Cut twice) (Metric input, Diameter programming)

G00 X 12.0 Z72.0 ;

Z axis

φ14

G32 X 41.0 Z29.0 F3.5 ; G00 X 50.0 ;

Z 72.0 ; X 10.0 ;

(Cut 1mm more for the second cut) G32 X 39.0 Z29.0 ; G00 X 50.0 ;

Z 72.0 ;

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62754EN/01

WARNING

1 Feedrate override is effective (fixed at 100%) during thread cutting. 2 it is very dangerous to stop feeding the thread cutter without stopping the spindle. This will

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

3 When the FEED HOLD button is held down, or is pressed again in the first block that does not

specify thread cutting immediately after a thread cutting block, the tool stops at the block that does not specify thread cutting.

4 When thread cutting is executed in the single block status, the tool stops after execution of the

first block not specifying thread cutting.

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

cutting, the tool stops at the first block not specifying thread cutting as when the feed hold button is pushed as mentioned in Note 3. However, when the mode is changed from one automatic operation mode to another, the tool stops after execution of the block not specifying thread cutting as for the single block mode in Note 4.

6 When the previous block was a thread cutting block, cutting will start immediately without

waiting for detection of the 1–turn signal even if the present block is a thread cutting block.

G32Z _ F_ ; Z _; (A 1–turn signal is not detected before this block.) G32 ; (Regarded as threading block.) Z_ F_ ;(One turn signal is also not detected.)

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

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

8 A movement block preceding the thread cutting block must not specify chamfering or corner

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

fixed at 100%. 11 Thread cycle retract function is ineffective to G32.

B–62754EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.9

VARIABLE–LEAD THREAD CUTTING (G34)

Format

Explanations

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

Fig. 4.9 (a) Variable–lead screw

G34 _F_K_;

 : End point F : Lead in long K : Increment and decrement of lead per spindle revolution

itudinal axis direction at the start point

Address other than K are the same as in straight/taper thread cutting with G32. Table 4.9 (a) lists a range of values that can be specified as K.

Examples

Table 4.9 (a) Range of valid K values

Metric input 0.0001 to 500.0000 mm/rev

Inch input 0.000001 to9.999999 inch/rev

P/S alarm (No. 14) is produced, for example, when K such that the value in Table 4.9 (a) is exceeded is directed, the maximum value of lead is exceeded as a result of increase or decrease by K or the lead has a negative value.

WARNING

The “Thread Cutting Cycle Retract” is not effective for G34.

Lead at the start point: 8.0 mm Lead increment: 0.3 mm/rev

G34 Z–72.0 F8.0 K0.3 ;

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62754EN/01

4.10

CONTINUOUS THREAD CUTTING

Explanations

This function for continuous thread cutting is such that fractional pulses output to a joint between move blocks are overlapped with the next move for pulse processing and output (block overlap) . Therefore, discontinuous machining sections caused by the interruption of move during continuously block machining are eliminated, thus making it possible to continuously direct the block for thread cutting instructions.

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

G32

Fig. 4.10 (a) Continuous Thread Cutting

G32

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

NOTE

1 Block overlap is effective even for G01 command,

producing a more excellent finishing surface.

2 When extreme micro blocks continue, no block overlap may

function.

B–62754EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.1 1

MUL TIPLE–THREAD CUTTING

Format

Explanations

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

Multiple–thread screws.

(constant–lead threading)

G32 IP_ F_ Q_ ; G32 IP_ Q_ ;

_ : End point

F_ : Lead in longitudinal direction Q_ : Threading start angle

D Available thread cutting

commands

Limitations

D Start angle

Start angle increment

D Specifiable start angle

range

D Multiple–thread cutting

(G76)

G32: Constant–lead thread cutting G34: Variable–lead thread cutting G76: Multiple–thread cutting cycle G92: Thread cutting cycle

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

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

A start angle (Q) of between 0 and 360000 (in 0.001–degree units) can be specified. If a value greater than 360000 (360 degrees) is specified, it is rounded down to 360000 (360 degrees).

For the G76 multiple–thread cutting command, always use the FS15 tape format.

4. INTERPOLA TION FUNCTIONS

Examples

PROGRAMMING

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

G00 X40.0 ; G32 W–38.0 F4.0 Q0 ; G00 X72.0 ;

W38.0 ;

X40.0 ; G32 W–38.0 F4.0 Q180000 ; G00 X72.0 ;

W38.0 ;

B–62754EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.12

CIRCULAR THREADING (G35, G36)

Format

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

Circular thread

G35 G36

X (U) _ Z (W) _ F _ Q _

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

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

G03).

Z (W)

I _ K _ R _ _ _

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

relative coordinates (in the same way as for G02, G03). R : Specify the arc radius. F : Specify the lead in the direction of the major axis. Q : Specify the shift of the threading start angle (0 to 360°

in units of 0.001°)

Start point

End point (Z, X)

Arc center

4. INTERPOLA TION FUNCTIONS

Explanations

PROGRAMMING

B–62754EN/01

D Specifying the arc radius D Selecting a plane other

than the ZX plane

D Automatic tool

compensation

If R is specified with I and K, only R is effective. If an additional axis other than the X– and Z–axes is provided, circular

threading can be specified for a plane other than the ZX plane. The method of specification is the same as that for G02 and G03.

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

D When parameter G36 is set to 0, the G36 command is used for

automatic tool compensation X.

D When parameter G36 is set to 1, the G36 command is used for

counterclockwise circular threading.

Automatic tool compensation using G37.1/G37.2

G37.1 can be used to specify automatic tool compensation X and G37.2 can be used to specify automatic tool compensation Z.

(Specification method) G37.1 X_ G37.2 Z_

G code when bit 3 of parameter No. 3405 is set to 1

G code G code group Function

G35 G36

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

Clockwise circular threading Counterclockwise circular threading

Automatic tool compensation X

B–62754EN/01

Limitations

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

D Range of specifiable arc

An arc must be specified such that it falls within a range in which the major axis of the arc is always the Z–axis or always the X–axis, as shown in Fig. 4.12 (a) and (b). If the arc includes a point at which the major axis changes from the X–axis to Z–axis, or vice versa, as shown in Fig. 4.12 (c), P/S alarm 5058 is issued.

Start point

Fig. 4.12 (a) Range in which the Z–axis is the major axis

End point

45°

Start point

45°

End point

Fig. 4.12 (b) Range in which the X–axis is the major axis

Start point

45°

The major axis changes at this point.

End point

Fig. 4.12 (c) Example of arc specification which causes an alarm

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62754EN/01

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. For details of how to use this function, refer to the manual supplied by the machine tool builder.

G31 _ ;

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 #5068, as follows:

#5061 X axis coordinate value #5062 Z axis coordinate value #5063 3rd axis coordinate value : : #5068 8th axis coordinate value

WARNING

To increase the precision of the tool position when the skip signal is input, feedrate override, dry run, and automatic acceleration/deceleration is disabled for the skip function when the feedrate is specified as a feed per minute value. To enable these functions, set bit 7 (SKF) of parameter No. 6200 to 1. If the feedrate is specified as a feed per rotation value, feedrate override, dry run, and automatic acceleration/deceleration are enabled for the skip function, regardless of the setting of the SKF bit.

NOTE

1 If G31 command is issued while tool nose radius compensation 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.

2 For the high–speed skip option, executing G31 during feed–per–

rotation mode causes P/S alarm 211 to be generated.

B–62754EN/01

Examples

D The next block to G31 is an

incremental command

PROGRAMMING

G31 W100.0 F100;

U50.0;

4. INTERPOLA TION FUNCTIONS

U50.0

D The next block to G31 is an

absolute command for 1 axis

Skip signal is input here

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

G31 Z200.00 F100;

X100.0;

Skip signal is input here

100.0

50.0

W100

Actual motion Motion without skip signal

X100.0

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 Z100.0;

Skip signal is input here

10 0

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

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62754EN/01

4.14

MULTISTAGE SKIP

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  __ F __ P __ ;

_ : 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.

B–62754EN/01

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.15

TORQUE LIMIT SKIP (G31 P99)

Format

Explanations

D G31 P99

With the motor torque limited (for example, by a torque limit command, issued through the PMC window), a move command following G31 P99 (or G31 P98) can cause the same type of cutting feed as with G01 (linear interpolation). With the issue of a signal indicating a torque limit has been reached (because of pressure being applied or for some other reason), a skip occurs. For details of how to use this function, refer to the manuals supplied by the machine tool builder.

G31 P99 IP_ F_ ; G31 P98 IP_ F_ ;

G31: One–shot G code (G code effective only in the block in which it is issued)

If the motor torque limit is reached, or a SKIP signal is received during execution of G31 P99, the current move command is aborted, and the next block is executed.

D G31 P98

D Torque limit command

D Custom macro system

variable

Limitations

D Axis command

If the motor torque limit is reached during execution of G31 P98, the current move command is aborted, and the next block is executed. The SKIP signal <X0004#7/Tool post 2 X0013#7> does not affect G31 P98. Entering a SKIP signal during the execution of G31 P98 does not cause a skip.

If a torque limit is not specified before the execution of G31 P99/98, the move command continues; no skip occurs even if a torque limit is reached.

When G31 P99/98 is specified, the custom macro variables hold the coordinates at the end of a skip. (See Section 4.9.) If a SKIP signal causes a skip with G31 P99, the custom macro system variables hold the coordinates based on the machine coordinate system when it stops, rather than those when the SKIP signal is entered.

Only one axis can be controlled in each block with G31 P98/99. If two or more axes are specified to be controlled in such blocks, or no axis command is issued, P/S alarm No. 015 is generated.

D Degree of servo error

D High–speed skip

When a signal indicating that a torque limit has been reached is input during execution of G31 P99/98, and the degree of servo error exceeds 32767, P/S alarm No. 244 is generated.

With G31 P99, a SKIP signal can cause a skip, but not a high–speed skip.

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62754EN/01

D Simplified

synchronization and slanted axis control

D Speed control

D Consecutive commands

G31 P99/98 cannot be used for axes subject to simplified synchronization or the X–axis or Z–axis when under slanted axis control.

Bit 7 (SKF) of parameter No. 6200 must be set to disable dry run, override, and auto acceleration or deceleration for G31 skip commands.

Do not use G31 P99/98 in consecutive blocks.

WARNING

Always specify a torque limit before a G31 P99/98 command. Otherwise, G31 P99/98 allows move commands to be executed without causing a skip.

NOTE

If G31 is issued with tool nose radius compensation specified, P/S alarm No. 035 is generated. Therefore, before issuing G31, execute G40 to cancel tool nose radius compensation.

Examples

O0001 ;

: : MJJ ; : : G31 P99 X200. F100 ; : G01 X100. F500 ; : : MYY ; : : M30 ; : %

The PMC specifies the torque limit through the window.

Torque limit skip command Move command for which a torque

limit is applied

Torque limit canceled by the PMC

B–62754EN/01

PROGRAMMING

 

5. FEED FUNCTIONS

PROGRAMMING

B–62754EN/01

5.1

GENERAL

D Feed functions

D Override

D Automatic acceleration/

deceleration

The feed functions control the feedrate of the tool. The following two feed functions are available:

1. Rapid traverse When the positioning command (G00) is specified, the tool moves at!a rapid traverse feedrate set in the CNC (parameter No. 1420).

2. Cutting feed The tool moves at a programmed cutting feedrate.

Override can be applied to a rapid traverse rate or cutting feedrate using the switch on the machine operator’s panel.

T o prevent a mechanical shock, acceleration/deceleration is automatically applied when the tool starts and ends its movement (Fig. 5.1 (a)).

Rapid traverse rate

:Rapid traverse

rate

: Acceleration/

deceleration time constant for rapid traverse rate

Time

Feed rate

Fig. 5.1 (a) Automatic acceleration/deceleration (example)

: Feedrate

: Acceleration/

deceleration time constant for a cutting feedrate

Time

B–62754EN/01

PROGRAMMING

5. FEED FUNCTIONS

D Tool path in a cutting

feed

If the direction of movement changes between specified blocks during cutting feed, a rounded–corner path may result (Fig. 5.1 (b)).

Programmed path Actual tool path

Fig. 5.1 (b) Example of Tool Path between Two Blocks

In circular interpolation, a radial error occurs (Fig. 5.1(c)).

∆r:Error

Programmed path Actual tool path

Fig. 5.1 (c) Example of Radial Error in Circular Interpolation

The rounded–corner path shown in Fig. 5.1(b) and the error shown in Fig.

5.1(c) depend on the feedrate. So, the feedrate needs to be controlled for

the tool to move as programmed.

5. FEED FUNCTIONS

5.2

RAPID TRAVERSE

Format

PROGRAMMING

G00 _ ;

G00 : G code (group 01) for positioning (rapid traverse) _ ; Dimension word for the end point

B–62754EN/01

Explanations

The positioning command (G00) positions the tool by rapid traverse. In rapid traverse, the next block is executed after the specified feedrate becomes 0 and the servo motor reaches a certain range set by the machine tool builder (in–position check). A rapid traverse rate is set for each axis by parameter No. 1420, so no rapid traverse feedrate need be programmed. The following overrides can be applied to a rapid traverse rate with the switch on the machine operator’s panel:F0, 25, 50, 100% F0: Allows a fixed feedrate to be set for each axis by parameter No. 1421. For detailed information, refer to the appropriate manual of the machine tool builder.

B–62754EN/01

PROGRAMMING

5. FEED FUNCTIONS

5.3

CUTTING FEED

Format

Explanations

Feedrate of linear interpolation (G01), circular interpolation (G02, G03), etc. are commanded with numbers after the F code. In cutting feed, the next block is executed so that the feedrate change from the previous block is minimized. Two modes of specification are available:

1. Feed per minute (G98) After F, specify the amount of feed of the tool per minute.

2. Feed per revolution (G99) After F, specify the amount of feed of the tool per spindle revolution.

Feed per minute

G98 ; G code (group 05) for feed per minute F_ ; Feedrate command (mm/min or inch/min)

Feed per revolution

G99 ; G code (group 05) for feed per revolution F_ ; Feedrate command (mm/rev or inch/rev)

D Tangential speed

constant control

D Feed per minute (G98)

Cutting feed is controlled so that the tangential feedrate is always set at a specified feedrate.

End point

Start point

Linear interpolation

Fig. 5.3 (a) T angential feedrate (F)

Starting point

Center

Circular interpolation

End point

After specifying G98 (in the feed per minute mode), the amount of feed of the tool per minute is to be directly specified by setting a number after F . G98 is a modal code. Once a G98 is specified, it is valid until G99 (feed per revolution) is specified. At power–on, the feed per revolution mode is set. An override from 0% to 254% (in 1% steps) can be applied to feed per minute with the switch on the machine operator’s panel. For detailed information, see the appropriate manual of the machine tool builder.

5. FEED FUNCTIONS

PROGRAMMING

B–62754EN/01

D Feed per revolution

(G99)

Fig. 5.3 (b) Feed per minute

Feed amount per minute (mm/min or inch/min)

WARNING

No override can be used for some commands such as for threading.

After specifying G99 (in the feed per revolution mode), the amount of feed of the tool per spindle revolution is to be directly specified by setting a number after F . G99 is a modal code. Once a G99 is specified, it is valid until G98 (feed per minute) is specified. An override from 0% to 254% (in 1% steps) can be applied to feed per revolution with the switch on the machine operator’s panel. For detailed information, see the appropriate manual of the machine tool builder.

If bit 0 (NPC) of parameter No. 1402 has been set to 1, feed–per–rotation commands can be specified even when a position coder is not being used. (The CNC converts feed–per–rotation commands to feed–per–minute commands.)

Fig. 5.3 (c) Feed per revolution

Feed amount per spindle revolution (mm/rev or inch/rev)

CAUTION

When the speed of the spindle is low, feedrate fluctuation may occur. The slower the spindle rotates, the more frequently feedrate fluctuation occurs.

D Cutting feedrate clamp

A common upper limit can be set on the cutting feedrate along each axis with parameter No. 1422. If an actual cutting feedrate (with an override applied) exceeds a specified upper limit, it is clamped to the upper limit.

fanuc 16C, 160C, 18C, 180-C Operator 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

PART DRAWING AND TOOL MOVEMENT

Coordinate system

PROGRAM CONFIGURATION

TOOL FIGURE AND TOOL MOTION BY PROGRAM

CONTROLLED AXES

CONTROLLED AXES

INCREMENT SYSTEM

INTERPOLATION FUNCTIONS

POSITIONING (G00)

CONSTANT LEAD THREADING (G32)

CONTINUOUS THREAD CUTTING

CIRCULAR THREADING (G35, G36)

TORQUE LIMIT SKIP (G31 P99)

GENERAL

RAPID TRAVERSE

CUTTING FEED