fanuc 21MB, 210–MB Operator’s Manual

Download

GE Fanuc Automation

Computer Numerical Control Products

Series 21 / 210–MB for Machining Center

Operator's Manual

GFZ-62704EN/03 September 1997

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.

PowerMotion is a trademark of GE Fanuc Automation North America, Inc.

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–62704EN/03

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–62704EN/03

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–62704EN/03

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–62704EN/03

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–62704EN/03

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–62704EN/03

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–62704EN/03

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–62704EN/03

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 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–62704EN/03

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 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–62704EN/03

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–11

B–62704EN/03

Table of Contents

SAFETY PRECAUTIONS s–1. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

I. GENERAL

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

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

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

II. PROGRAMMING

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

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

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

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

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

1.3.2 Coordinate System on Part Drawing and Coordinate System Specified by

1.3.3 How to Indicate Command Dimensions for Moving the Tool – Absolute, Incremental Commands 19. . . . .

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

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

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

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

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

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

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

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

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

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

2.3 INCREMENT SYSTEM 30. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4 MAXIMUM STROKE 30. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3. PREPARATORY FUNCTION (G FUNCTION) 31. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4. INTERPOLATION FUNCTIONS 36. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.1 POSITIONING (G00) 37. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.2 SINGLE DIRECTION POSITIONING (G60) 39. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.3 LINEAR INTERPOLATION (G01) 41. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.4 CIRCULAR INTERPOLATION (G02,G03) 43. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.5 HELICAL INTERPOLATION (G02,G03) 47. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.6 CYLINDRICAL INTERPOLATION (G07.1) 48. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.7 THREAD CUTTING (G33) 51. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8 SKIP FUNCTION(G31) 53. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5. FEED FUNCTIONS 55. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.1 GENERAL 56. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.2 RAPID TRAVERSE 58. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–1

Table of Contents

B–62704EN/03

5.3 CUTTING FEED 59. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4 CUTTING FEEDRATE CONTROL 62. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.1 Exact Stop (G09, G61) Cutting Mode (G64) Tapping Mode (G63) 63. . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.2 Automatic Corner Override 64. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.2.1 Automatic Override for Inner Corners (G62) 64. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.2.2 Internal Circular Cutting Feedrate Change 67. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.5 DWELL (G04) 68. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6. REFERENCE POSITION 69. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.1 REFERENCE POSITION RETURN 70. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7. COORDINATE SYSTEM 74. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1 MACHINE COORDINATE SYSTEM 75. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2 WORKPIECE COORDINATE SYSTEM 76. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.1 Setting a Workpiece Coordinate System 76. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.2 Selecting a Workpiece Coordinate System 77. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.3 Changing Workpiece Coordinate System 78. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.4 Workpiece coordinate system preset (G92.1) 81. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.5 Adding Workpiece Coordinate Systems (G54.1 or G54) 83. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.3 LOCAL COORDINATE SYSTEM 85. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.4 PLANE SELECTION 87. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8. COORDINATE VALUE AND DIMENSION 88. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1 ABSOLUTE AND INCREMENTAL PROGRAMMING (G90, G91) 89. . . . . . . . . . . . . . . . . . . . . . .

8.2 POLAR COORDINATE COMMAND (G15, G16) 90. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3 INCH/METRIC CONVERSION (G20,G21) 93. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4 DECIMAL POINT PROGRAMMING 94. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9. SPINDLE FUNCTION (S FUNCTION) 95. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1 SPECIFYING THE SPINDLE SPEED WITH A CODE 96. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2 SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY (S5–DIGIT COMMAND) 96. . . . . . . . .

9.3 CONSTANT SURFACE SPEED CONTROL (G96, G97) 97. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.TOOL FUNCTION (T FUNCTION) 100. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.1 TOOL SELECTION FUNCTION 101. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2 TOOL LIFE MANAGEMENT FUNCTION 102. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2.1 Tool Life Management Data 103. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2.2 Register, Change and Delete of Tool Life Management Data 104. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2.3 Tool Life Management Command in a Machining Program 107. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2.4 Tool Life 110. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.AUXILIARY FUNCTION 111. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1 AUXILIARY FUNCTION (M FUNCTION) 112. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2 MULTIPLE M COMMANDS IN A SINGLE BLOCK 113. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3 THE SECOND AUXILIARY FUNCTIONS (B CODES) 114. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–2

B–62704EN/03

Table of Contents

12.PROGRAM CONFIGURATION 115. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.1 PROGRAM COMPONENTS OTHER THAN PROGRAM SECTIONS 117. . . . . . . . . . . . . . . . . . . . . .

12.2 PROGRAM SECTION CONFIGURATION 120. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.3 SUBPROGRAM (M98, M99) 126. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.FUNCTIONS TO SIMPLIFY PROGRAMMING 130. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1 CANNED CYCLE 131. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.1 High–speed Peck Drilling Cycle (G73) 135. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.2 Left–handed Tapping Cycle (G74) 137. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.3 Fine Boring Cycle (G76) 139. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.4 Drilling Cycle, Spot Drilling (G81) 141. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.5 Drilling Cycle Counter Boring Cycle (G82) 143. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.6 Peck Drilling Cycle (G83) 145. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.7 Small–hole peck drilling cycle (G83) 147. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.8 Tapping Cycle (G84) 151. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.9 Boring Cycle (G85) 153. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.10 Boring Cycle (G86) 155. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.11 Boring Cycle Back Boring Cycle (G87) 157. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.12 Boring Cycle (G88) 159. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.13 Boring Cycle (G89) 161. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.14 Canned Cycle Cancel (G80) 163. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.2 RIGID TAPPING 166. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.2.1 Rigid Tapping (G84) 167. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.2.2 Left–handed Rigid Tapping Cycle (G74) 170. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.2.3 Peck Rigid Tapping Cycle (G84 or G74) 173. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.2.4 Canned Cycle Cancel (G80) 175. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.3 OPTIONAL ANGLE CHAMFERING AND CORNER ROUNDING 176. . . . . . . . . . . . . . . . . . . . . . . .

13.4 EXTERNAL MOTION FUNCTION (G81) 179. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.5 INDEX TABLE INDEXING FUNCTION 180. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.COMPENSATION FUNCTION 183. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1 TOOL LENGTH OFFSET (G43,G44,G49) 184. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.1 General 184. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.2 G53, G28, and G30 Commands in Tool Length Offset Mode 189. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2 AUTOMATIC TOOL LENGTH MEASUREMENT (G37) 192. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3 TOOL OFFSET (G45–G48) 196. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4 OVERVIEW OF CUTTER COMPENSATION C (G40 – G42) 201. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5 DETAILS OF CUTTER COMPENSATION C 207. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.1 General 207. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.2 Tool Movement in Start–up 208. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.3 Tool Movement in Offset Mode 212. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.4 Tool Movement in Offset Mode Cancel 226. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.5 Interference Check 232. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.6 Overcutting by Cutter Compensation 237. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.7 Input Command from MDI 240. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.8 G53,G28,G30,G30.1 and G29 Commands in Cutter Compensation C Mode 241. . . . . . . . . . . . . . . . . . . .

14.5.9 Corner Circular Interpolation (G39) 260. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

AND ENTERING VALUES FROM THE PROGRAM (G10) 262. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.7 SCALING (G50,G51) 264. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.8 COORDINATE SYSTEM ROTATION (G68, G69) 269. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–3

Table of Contents

B–62704EN/03

14.9 NORMAL DIRECTION CONTROL (G40.1, G41.1, G42.1 OR G150, G151, G152) 275. . . . . . . . . . . .

14.10 PROGRAMMABLE MIRROR IMAGE (G50.1, G51.1) 280. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.CUSTOM MACRO 282. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1 V ARIABLES 283. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2 SYSTEM VARIABLES 287. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3 ARITHMETIC AND LOGIC OPERATION 295. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.4 MACRO STATEMENTS AND NC STATEMENTS 300. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.5 BRANCH AND REPETITION 301. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.5.1 Unconditional Branch (GOTO Statement) 301. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.5.2 Conditional Branch (IF Statement) 302. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.5.3 Repetition (While Statement) 303. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6 MACRO CALL 306. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.1 Simple Call (G65) 307. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.2 Modal Call (G66) 311. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.3 Macro Call Using G Code 313. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.4 Macro Call Using an M Code 314. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.5 Subprogram Call Using an M Code 315. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.6 Subprogram Calls Using a T Code 316. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.7 Sample Program 317. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.7 PROCESSING MACRO ST ATEMENTS 319. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.8 REGISTERING CUSTOM MACRO PROGRAMS 321. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.9 LIMITATIONS 322. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.10 EXTERNAL OUTPUT COMMANDS 323. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.11 INTERRUPTION TYPE CUSTOM MACRO 327. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.11.1 Specification Method 328. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.11.2 Details of Functions 329. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.PATTERN DATA INPUT FUNCTION 336. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.1 DISPLAYING THE PATTERN MENU 337. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.2 P ATTERN DATA DISPLAY 341. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.3 CHARACTERS AND CODES TO BE USED

FOR THE PATTERN DATA INPUT FUNCTION 345. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

17.PROGRAMMABLE PARAMETER ENTRY (G10) 347. . . . . . . . . . . . . . . . . . . . . . . . . . .

18.MEMORY OPERATION USING FS10/11 TAPE FORMAT 349. . . . . . . . . . . . . . . . . . .

19.HIGH SPEED CUTTING FUNCTIONS 350. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19.1 FEEDRATE CLAMPING BY ARC RADIUS 351. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19.2 ADVANCED PREVIEW CONTROL (G08) 352. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19.3 HIGH–SPEED REMOTE BUFFER 354. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19.3.1 High–speed remote buffer A (G05) 354. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19.3.2 High–speed remote buffer B (G05) 357. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.AXIS CONTROL FUNCTIONS 358. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.1 SIMPLE SYNCHRONOUS CONTROL 359. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.2 ROTARY AXIS ROLL–OVER 362. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–4

B–62704EN/03

Table of Contents

III. OPERATION

1. GENERAL 365. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.1 MANUAL OPERATION 366. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.2 TOOL MOVEMENT BY PROGRAMMING– AUTOMATIC OPERATION 368. . . . . . . . . . . . . . . . . .

1.3 AUTOMATIC OPERATION 369. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4 TESTING A PROGRAM 371. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4.1 Check by Running the Machine 371. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4.2 How to View the Position Display Change without Running the Machine 372. . . . . . . . . . . . . . . . . . . . .

1.5 EDITING A PART PROGRAM 373. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.6 DISPLAYING AND SETTING DATA 374. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7 DISPLAY 377. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.1 Program Display 377. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.2 Current Position Display 378. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.3 Alarm Display 378. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.4 Parts Count Display, Run Time Display 379. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.5 Graphic Display 379. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.8 DATA INPUT / OUTPUT 380. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2. OPERATIONAL DEVICES 381. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1 CRT/MDI PANELS 382. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.2 EXPLANATION OF THE KEYBOARD 391. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3 FUNCTION KEYS AND SOFT KEYS 393. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.1 General Screen Operations 393. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.2 Function Keys 394. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.3 Soft Keys 395. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.4 Key Input and Input Buffer 411. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.5 Warning Messages 412. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.6 Soft Key Configuration 413. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4 EXTERNAL I/O DEVICES 414. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.1 FANUC Handy File 416. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.2 FANUC Floppy Cassette 416. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.3 FANUC FA Card 417. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.4 FANUC PPR 417. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.5 Portable Tape Reader 418. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5 POWER ON/OFF 419. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.1 Turning on the Power 419. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.2 Screen Displayed at Power–on 420. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.3 Power Disconnection 421. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3. MANUAL OPERATION 422. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.1 MANUAL REFERENCE POSITION RETURN 423. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.2 JOG FEED 425. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.3 INCREMENTAL FEED 427. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.4 MANUAL HANDLE FEED 428. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.5 MANUAL ABSOLUTE ON AND OFF 430. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4. AUTOMATIC OPERATION 435. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.1 MEMOR Y OPERATION 436. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–5

Table of Contents

B–62704EN/03

4.2 MDI OPERATION 439. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.3 DNC OPERATION 443. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.4 PROGRAM REST ART 446. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.5 SCHEDULING FUNCTION 453. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.6 SUBPROGRAM CALL FUNCTION (M198) 458. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.7 MANUAL HANDLE INTERRUPTION 460. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8 MIRROR IMAGE 463. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.9 MANUAL INTERVENTION AND RETURN 465. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5. TEST OPERATION 467. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.1 MACHINE LOCK AND AUXILIAR Y FUNCTION LOCK 468. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.2 FEEDRATE OVERRIDE 470. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.3 RAPID TRAVERSE OVERRIDE 471. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4 DRY RUN 472. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.5 SINGLE BLOCK 473. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6. SAFETY FUNCTIONS 475. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.1 EMERGENCY STOP 476. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.2 OVERTRAVEL 477. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.3 STROKE CHECK 478. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7. ALARM AND SELF–DIAGNOSIS FUNCTIONS 482. . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1 ALARM DISPLAY 483. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2 ALARM HISTORY DISPLAY 485. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.3 CHECKING BY SELF–DIAGNOSTIC SCREEN 486. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8. DATA INPUT/OUTPUT 489. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1 FILES 490. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2 FILE SEARCH 492. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3 FILE DELETION 493. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4 PROGRAM INPUT/OUTPUT 494. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.1 Inputting a Program 494. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.2 Outputting a Program 497. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5 OFFSET DATA INPUT AND OUTPUT 499. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5.1 Inputting Offset Data 499. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5.2 Outputting Offset Data 500. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6 INPUTTING AND OUTPUTTING PARAMETERS AND

PITCH ERROR COMPENSATION DATA 501. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.1 Inputting Parameters 501. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.2 Outputting Parameters 502. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.3 Inputting Pitch error compensation data 503. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.4 Outputting Pitch Error Compensation Data 504. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.7 INPUTTING/OUTPUTTING CUSTOM MACRO COMMON VARIABLES 505. . . . . . . . . . . . . . . . . .

8.7.1 Inputting Custom Macro Common Variables 505. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.7.2 Outputting Custom Macro Common Variable 506. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8 DISPLAYING DIRECTORY OF FLOPPY CASSETTE 507. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.1 Displaying the Directory 508. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–6

B–62704EN/03

8.8.2 Reading Files 511. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.3 Outputting Programs 512. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.4 Deleting Files 513. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Table of Contents

8.9 OUTPUTTING A PROGRAM LIST FOR A SPECIFIED GROUP 515. . . . . . . . . . . . . . . . . . . . . . . . .

8.10 DATA INPUT/OUTPUT ON THE ALL IO SCREEN 516. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.10.1 Setting Input/Output–Related Parameters 517. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.10.2 Inputting and Outputting Programs 518. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.10.3 Inputting and Outputting Parameters 523. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.10.4 Inputting and Outputting Offset Data 525. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.10.5 Outputting Custom Macro Common Variables 527. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.10.6 Inputting and Outputting Floppy Files 528. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9. EDITING PROGRAMS 533. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1 INSERTING, ALTERING AND DELETING A WORD 534. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.1 Word Search 535. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.2 Heading a Program 537. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.3 Inserting a Word 538. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.4 Altering a Word 539. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.5 Deleting a Word 540. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2 DELETING BLOCKS 541. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.1 Deleting a Block 541. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.2 Deleting Multiple Blocks 542. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3 PROGRAM NUMBER SEARCH 543. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4 SEQUENCE NUMBER SEARCH 544. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5 DELETING PROGRAMS 546. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.1 Deleting One Program 546. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.2 Deleting All Programs 546. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.3 Deleting More Than One Program by Specifying a Range 547. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6 EXTENDED PART PROGRAM EDITING FUNCTION 548. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.1 Copying an Entire Program 549. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.2 Copying Part of a Program 550. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.3 Moving Part of a Program 551. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.4 Merging a Program 552. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.5 Supplementary Explanation for Copying,Moving and Merging 553. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.6 Replacement of Words and Addresses 555. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.7 EDITING OF CUSTOM MACROS 557. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.8 BACKGROUND EDITING 558. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.9 PASSWORD FUNCTION 559. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.CREATING PROGRAMS 561. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.1 CREATING PROGRAMS USING THE MDI P ANEL 562. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2 AUTOMATIC INSERTION OF SEQUENCE NUMBERS 563. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.3 CREATING PROGRAMS IN TEACH IN MODE (PLA YBACK) 565. . . . . . . . . . . . . . . . . . . . . . . . . . .

11.SETTING AND DISPLAYING DATA 568. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1 SCREENS DISPLAYED BY FUNCTION KEY

11.1.1 Position Display in the Work Coordinate System 576. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.2 Position Display in the Relative Coordinate System 577. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.3 Overall Position Display 579. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.4 Presetting the Workpiece Coordinate System 580. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

POS

c–7

575. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Table of Contents

B–62704EN/03

11.1.5 Actual Feedrate Display 581. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.6 Display of Run Time and Parts Count 583. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.7 Operating Monitor Display 584. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2 SCREENS DISPLAYED BY FUNCTION KEY

PROG

(IN MEMORY MODE OR MDI MODE) 586. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.1 Program Contents Display 587. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.2 Current Block Display Screen 588. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.3 Next Block Display Screen 589. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.4 Program Check Screen 590. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.5 Program Screen for MDI Operation 592. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3 SCREENS DISPLAYED BY FUNCTION KEY

11.3.1 Displaying Memory Used and a List of Programs 593. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3.2 Displaying a Program List for a Specified Group 597. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4 SCREENS DISPLAYED BY FUNCTION KEY

11.4.1 Setting and Displaying the Tool Offset Value 601. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.2 Tool Length Measurement 604. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.3 Displaying and Entering Setting Data 606. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.4 Sequence Number Comparison and Stop 608. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.5 Displaying and Setting Run Time,Parts Count, and Time 610. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.6 Displaying and Setting the Workpiece Origin Offset Value 612. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.7 Direct Input of Measured Workpiece Origin Offsets 613. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.8 Displaying and Setting Custom Macro Common Variables 615. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.9 Displaying Pattern Data and Pattern Menu 616. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.10 Displaying and Setting the Software Operator’s Panel 618. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.11 Displaying and Setting Tool Life Management Data 620. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.12 Displaying and Setting Extended Tool Life Management 623. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

PROG

(IN THE EDIT MODE) 593. . . . . . . . . . . . . . . .

OFFSET SETTING

600. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5 SCREENS DISPLAYED BY FUNCTION KEY

SYSTEM

11.5.1 Displaying and Setting Parameters 629. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5.2 Displaying and Setting Pitch Error Compensation Data 631. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.6 DISPLA YING THE PROGRAM NUMBER, SEQUENCE NUMBER, AND STATUS,

AND WARNING MESSAGES FOR DATA SETTING OR INPUT/OUTPUT OPERATION 633. . . . . .

11.6.1 Displaying the Program Number and Sequence Number 633. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.6.2 Displaying the Status and Warning for Data Setting or Input/Output Operation 634. . . . . . . . . . . . . . . . .

11.7 SCREENS DISPLAYED BY FUNCTION KEY

MESSAGE

11.7.1 External Operator Message History Display 636. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8 CLEARING THE SCREEN 638. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8.1 Erase Screen Display 638. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8.2 Automatic Erase Screen Display 639. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.GRAPHICS FUNCTION 640. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.1 GRAPHICS DISPLAY 641. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.2 DYNAMIC GRAPHIC DISPLA Y 647. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.2.1 Path Drawing 647. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.HELP FUNCTION 656. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

628. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

636. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–8

B–62704EN/03

Table of Contents

IV. MAINTENANCE

1. METHOD OF REPLACING BATTERY 663. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.1 REPLACING CNC BATTERY FOR MEMORY BACK–UP 664. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.2 REPLACING BATTERIES FOR ABSOLUTE PULSE CODER 666. . . . . . . . . . . . . . . . . . . . . . . . . . .

1.3 REPLACING BATTERIES FOR ABSOLUTE PULSE CODER

(α SERIES SERVO AMPLIFIER MODULE) 667. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

APPENDIX

A. TAPE CODE LIST 671. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B. LIST OF FUNCTIONS AND TAPE FORMAT 674. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

C. RANGE OF COMMAND VALUE 680. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D. NOMOGRAPHS 683. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D.1 INCORRECT THREADED LENGTH 684. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D.2 SIMPLE CALCULATION OF INCORRECT THREAD LENGTH 686. . . . . . . . . . . . . . . . . . . . . . . . . .

D.3 TOOL PATH AT CORNER 688. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D.4 RADIUS DIRECTION ERROR AT CIRCLE CUTTING 691. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

E. STATUS WHEN TURNING POWER ON, WHEN CLEAR AND WHEN RESET 692. . .

F. CHARACTER–TO–CODES CORRESPONDENCE TABLE 694. . . . . . . . . . . . . . . . . .

G. ALARM LIST 695. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

H. OPERATION OF PORTABLE TAPE READER 715. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–9

I. GENERAL

B–62704EN/03

GENERAL

  

GENERAL

This manual consists of the following parts:

I. GENERAL

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

II. PROGRAMMING

Describes each function: Format used to program functions in the NC language, characteristics, and restrictions. When a program is created through conversational automatic programming function, refer to the manual for the conversational automatic programming function (Table 1).

III. OPERATION

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

IV. MAINTENANCE

Describes procedures for replacing batteries.

APPENDIX

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

1. GENERAL

Applicable models

Some functions described in this manual may not be applied to some products. For detail, refer to the DESCRIPTIONS manual(B–62702EN).

This manual does not describe parameters in detail. For details on parameters mentioned in this manual, refer to the manual for parameters (B–62710EN).

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 21–MB 21–MB Series 21 FANUC Series 210–MB 210–MB Series 210

1. GENERAL

GENERAL

B–62704EN/03

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 B of Series 21 and Series

210. In the table, this manual is marked with an asterisk (*).

T able 1 Related Manuals

Manual name

DESCRIPTIONS B–62702EN CONNECTION MANUAL (Hardware) B–62703EN CONNECTION MANUAL (Function) B–62703EN–1 OPERATOR’S MANUAL for Lathe B–62534E OPERATOR’S MANUAL for Machining Center B–62704EN

Specification

number

MAINTENANCE MANUAL B–62705 PARAMETER MANUAL B–62710EN PROGRAMMING MANUAL (Macro Compiler / Macro Executer) B–61803E–1 FAPT MACRO COMPILER PROGRAMMING MANUAL B–66102E CONVERSATIONAL AUTOMATIC PROGRAMMING FUNCTION I

FOR MACHINING CENTER OPERATOR’S MANUAL

B–61874E–1

B–62704EN/03

Machining rocess

GENERAL

1. GENERAL

1.1 GENERAL FLOW OF OPERATION OF CNC MACHINE TOOL

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

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

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

Part drawing

CHAPTER II PROGRAMMING CHAPTER III OPERATION

Part programming

CNC

MACHINE TOOL

Before the actual programming, make the machining plan for how to

machine the part. Machining plan

1. Determination of workpieces machining range

2. Method of mounting workpieces on the machine tool

3. Machining sequence in every machining process

4. Machining tools and machining

Decide the machining method in every machining process.

Machining process

Machining procedure

1. Machining method : Rough Semi Finish

2. Machining tools

3. Machining conditions : Feedrate Cutting depth

4. Tool path

1 2 3

Feed cutting Side cutting

Hole

machining

1. GENERAL

GENERAL

Tool

Side cutting

B–62704EN/03

Face cutting

Hole machining

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

B–62704EN/03

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–62704EN/03



PROGRAMMING

1. GENERAL

PROGRAMMING

B–62704EN/03

1.1 TOOL MOVEMENT ALONG WORKPIECE PARTS FIGURE– INTERPOLATION

Explanations

D Tool movement along a

straight line

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

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

Tool

Workpiece

Program G01 X_ _ Y_ _ ; X_ _ ;

D Tool movement along an

arc

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

Program G03X_ _Y_ _R_ _;

Tool

Workpiece

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

B–62704EN/03

PROGRAMMING

1. GENERAL

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

(a) Movement along straight line

G01 Y_ _; X– –Y– – – –;

Control unit

Interpolation

a)Movement

along straight line

b)Movement

along arc

Fig. 1.1 (c) Interpolation function

(b) Movement along arc

G03X––Y––R––;

X axis

Y axis

Tool movement

NOTE

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

1. GENERAL

PROGRAMMING

B–62704EN/03

1.2

FEED–FEED FUNCTION

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

mm/min

Workpiece

Table

Fig. 1.2 Feed function

Tool

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

B–62704EN/03

1.3 PART DRAWING AND TOOL MOVEMENT

PROGRAMMING

1. GENERAL

1.3.1

Reference Position (Machine–Specific Position)



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

Reference position

Tool

Workpiece

Table

Fig. 1.3.1 Reference position

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

Reference position return is performed by manual button operation.

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

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

1. GENERAL

1.3.2

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

PROGRAMMING

B–62704EN/03

Program

Explanations

D Coordinate system

Part drawing

Fig. 1.3.2 (a)

Coordinate system

CNC

Command

Tool

Workpiece

Machine tool

Coordinate system

The following two coordinate systems are specified at different locations: (See II–7)

(1)Coordinate system on part drawing

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

(2)Coordinate system specified by the CNC

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

230

300

Program zero point

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

Present tool position

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

B–62704EN/03

PROGRAMMING

1. GENERAL

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

Coordinate system on part drawing established on the work-

Coordinate system specified by the CNC established on the table

Table

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

systemon part drawing

Workpiece

piece

D Methods of setting the

two coordinate systems in the same position

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

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

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

Fixed distance

Program zero point

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

Workpiece’s standard point

Fixed distance

1. GENERAL

PROGRAMMING

B–62704EN/03

(2)Mounting a workpiece directly against the jig

Program zero point

Jig

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

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

pallet on the jig

Pallet

Jig

Workpiece

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

B–62704EN/03

1.3.3

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

PROGRAMMING

1. GENERAL

Explanations

D Absolute command

Command for moving the tool can be indicated by absolute command or incremental command (See II–8.1).

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

Command specifying movement from point A to point B



B(10.0,30.0,20.0)

G90 X10.0 Y30.0 Z20.0 ;

Coordinates of point B

Tool

D Incremental command

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

Tool

X=40.0



Z=–10.0

Command specifying movement from point A to point B

Y=–30.0

G91 X40.0 Y–30.0 Z–10.0

Distance and direction for movement along each axis

;

1. GENERAL

PROGRAMMING

B–62704EN/03

1.4 CUTTING SPEED – SPINDLE SPEED FUNCTION

Examples

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

Tool

Spindle speed N

rpm

Workpiece

Tool diameter  D mm

V: Cutting speed

m/min

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

S250; Commands related to the spindle speed are called the spindle speed function ( See II–9) .

B–62704EN/03

PROGRAMMING

1. GENERAL

1.5 SELECTION OF TOOL USED FOR VARIOUS MACHINING – TOOL FUNCTION

Examples

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

Tool number

01 02

When the tool is stored at location 01 in the ATC magazine, the tool can be selected by specifying T01. This is called the tool function (See II–10).

A TC magazine

1. GENERAL

PROGRAMMING

B–62704EN/03

1.6 COMMAND FOR MACHINE OPERATIONS – MISCELLANEOUS FUNCTION

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

Tool

Coolant

Workpiece

The function of specifying the on–off operations of the components of the machine is called the miscellaneous function. In general, the function is specified by an M code (See II–11). For example, when M03 is specified, the spindle is rotated clockwise at the specified spindle speed.

B–62704EN/03

PROGRAMMING

1. GENERAL

1.7

PROGRAM CONFIGURATION

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

Block

Tool movement sequence

Block

Program

Fig. 1.7 (a) Program configuration

Block

⋅ ⋅ ⋅ ⋅

Block

A group of commands at each step of the sequence is called the block. The program consists of a group of blocks for a series of machining. The number for discriminating each block is called the sequence number, and the number for discriminating each program is called the program number (See II–12).

1. GENERAL

PROGRAMMING

B–62704EN/03

Explanations

D Block

D Program

The block and the program have the following configurations.

1 block

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

Sequence number

Preparatory function

Dimension word Miscel-

laneous function

Fig. 1.7 (b) Block configuration

Spindle function

Tool function

End of block

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

;

Offff;

⋅ ⋅ ⋅

M30 ;

Fig. 1.7 (c) Program configuration

Program number

Block Block Block

⋅ ⋅ ⋅

End of program

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

B–62704EN/03

PROGRAMMING

1. GENERAL

D Main program and

subprogram

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

Main program

⋅ ⋅

M98P1001

⋅ ⋅ ⋅

M98P1002

⋅ ⋅ ⋅

M98P1001

⋅ ⋅

Subprogram #1

O1001

M99

Subprogram #2

O1002

Program for hole #1

Program for hole #2

⋅

M99

Hole #1

Hole #2

1. GENERAL

1.8

TOOL FIGURE AND TOOL MOTION BY PROGRAM

Explanations

PROGRAMMING

B–62704EN/03

D Machining using the end

of cutter – Tool length compensation function (See II–14.1)

D Machining using the side

of cutter – Cutter compensation function (See II–14.4,14.5)

Usually, several tools are used for machining one workpiece. The tools have different tool length. It is very troublesome to change the program in accordance with the tools. Therefore, the length of each tool used should be measured in advance. By setting the difference between the length of the standard tool and the length of each tool in the CNC (data display and setting : see III–11), machining can be performed without altering the program even when the tool is changed. This function is called tool length compensation.

Standard tool

Workpiece

H3 H4

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

Cutter path using cutter compensation

Machined part figure

Workpiece

Cutter

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

B–62704EN/03

PROGRAMMING

1. GENERAL

1.9

TOOL MOVEMENT RANGE – STROKE

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

Table

Motor

Limit switch

Machine zero point

Specify these distances.

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

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

2. CONTROLLED AXES

CONTROLLED AXES

PROGRAMMING

B–62704EN/03

2.1 CONTROLLED AXES

PROGRAMMING

2. CONTROLLED AXES

2.2 AXIS NAME

Limitations

Item

No. of basic controlled axes 3 axes Controlled axes expansion (total) Max. 4 axes (included in Cs axis) Basic simultaneously controlled axes 2 axes Simultaneously controlled axes

expansion (total)

Max. 4 axes

21–MB

210–MB

NOTE

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

The names of three basic axes are always X, Y, and Z. The name of an additional axis can be set to A, B, C, U, V, or W by using parameter 1020. Parameter No. 1020 is used to determine the name of each axis.

D Default axis name

D Duplicate axis names

Each axis is named as specified in parameter No. 1020. If the parameter is 0, or it specifies invalid characters (such as nonalphabetic), the axes are named 1, 2, 3, and 4 by default. When a default axis name (1 to 4) is used, operation in the MEM mode and MDI mode is disabled.

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

2. CONTROLLED AXES

IS–B

IS–C

PROGRAMMING

B–62704EN/03

2.3 INCREMENT SYSTEM

The increment system consists of the least input increment (for input) and least command increment (for output). The least input increment is the least increment for programming the travel distance. The least command increment is the least increment for moving the tool on the machine. Both increments are represented in mm, inches, or deg. There are two increment systems: IS–B and IS–C. Which to use is selected according to the ISC parameter (bit 1 of parameter No. 1004). If IS–C is selected, it requires an option that supports 1/10 of the increment system. The setting of the ISC parameter (bit 1 of parameter No. 1004) applies to all axes. If IS–C is selected, for example, the increment system for any axis is assumed to be IS–C.

Name of increment system

IS–B

Name of increment system

IS–C

Least input increment

0.001mm

0.0001inch

0.001deg Least input incre-

ment

0.0001mm

0.00001inch

0.0001deg

Least command increment

0.001mm

0.0001inch

0.001deg Least command

increment

0.0001mm

0.00001inch

0.0001deg

Maximum stroke

99999.999mm

9999.9999inch

99999.999deg Maximum

stroke

9999.9999mm

999.99999inch

9999.9999deg

2.4 MAXIMUM STROKE

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

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

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

T able 2.4 Maximum strokes

Increment system

Metric machine system 99999.999 mm

–

Inch machine system 9999.9999 inch

Metric machine system 9999.9999 mm

–

Inch machine system 999.99999 inch

Maximum stroke

99999.999 deg

9999.9999 deg

NOTE

1 A command exceeding the maximum stroke cannot be

specified.

2 The actual stroke depends on the machine tool.

B–62704EN/03

3. PREP ARATORY FUNCTION

PROGRAMMING

PREPARATORY FUNCTION (G FUNCTION)

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

Type Meaning

One–shot G code The G code is effective only in the block in which it is

specified.

Modal G code The G code is effective until another G code of the

same group is specified.

(Example ) G01 and G00 are modal G codes in group 01.

(G FUNCTION)

G01X 

Z X

G00Z

G01 is effective in this range.



3. PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING

B–62704EN/03

Explanations

1. When the clear state (bit 6 (CLR) of parameter No. 3402) is set at power–up or reset, the modal G codes are placed in the states described below.

(1) The modal G codes are placed in the states marked with

indicated in Table 3.

(2) G20 and G21 remain unchanged when the clear state is set at

power–up or reset.

(3) Which status G22 or G23 at power on is set by parameter G23 (No.

3402#7). However, G22 and G23 remain unchanged when the clear state is set at reset.

(4) The user can select G00 or G01 by setting bit 0 (G01) of parameter

No. 3402.

(5) The user can select G90 or G91 by setting bit 3 (G91) of parameter

No. 3402.

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

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

2.G codes other than G10 and G11 are one–shot G codes.

3.When a G code not listed in the G code list is specified, or a G code that has no corresponding option is specified, P/S alarm No. 010 is output.

4.Multiple G codes can be specified in the same block if each G code belongs to a different group. If multiple G codes that belong to the same group are specified in the same block, only the last G code specified is valid.

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

6.G codes are indicated by group.

7.The group of G60 is switched according to the setting of the MDL bit (bit 0 of parameter 5431). (When the MDL bit is set to 0, the 00 group is selected. When the MDL bit is set to 1, the 01 group is selected.)

B–62704EN/03

3. PREP ARATORY FUNCTION

PROGRAMMING

T able 3 G code list (1/3)

G code

G00 G01 G02 G03 Circular interpolation/Helical interpolation CCW G04 Dwell, Exact stop G05 High speed cycle machining G07 Hypothetical axis interpolation G07.1 (G107) G08 G09 Exact stop G10 Programmable data input G11 Programmable data input mode cancel

G15 G16

G17

G18

G19 G20 G21

G22 G23

G25 G26 G27 Reference position return check G28 Return to reference position G29 00 Return from reference position G30 2nd, 3rd and 4th reference position return G31 Skip function G33 01 Thread cutting G37 00 Automatic tool length measurment G40 G41 G42 Cutter compensation right

G40.1 (G150) G41.1 (G151) 19 Normal direction control left side on

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

G47 G48 Tool offset double decrease

Group Function

Positioning

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

Linear interpolation Circular interpolation/Helical interpolation CW

Cylindrical interpolation Look–ahead control

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

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

Cutter compensation cancel Cutter compensation left

Normal direction control cancel mode

Tool length compensation + direction Tool length compensation – direction

Tool offset decrease Tool offset double increase

(G FUNCTION)

3. PREPARATORY FUNCTION

(G FUNCTION)

G code FunctionGroup

G49 G50 G51 G50.1 G51.1 G52 G53 G54 G54.1 Additional workpiece coordinate system selection

G55 G56 G57 Workpiece coordinate system 4 selection G58 Workpiece coordinate system 5 selection G59 Workpiece coordinate system 6 selection G60 00 Single direction positioning G61 Exact stop mode G62 G63 G64 G65 00 Macro call G66

G67 G68

G69 G73 Peck drilling cycle G74 Counter tapping cycle G76 Fine boring cycle

G80 G81

G82 Drilling cycle or counter boring cycle G83 G84 Tapping cycle G85 Boring cycle G86 Boring cycle G87 Back boring cycle G88 Boring cycle G89 Boring cycle G90 G91

G92 G92.1 Workpiece coordinate system preset

PROGRAMMING

T able 3 G code list (2/3)

08 Tool length compensation cancel

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

Workpiece coordinate system 2 selection

Workpiece coordinate system 3 selection

Automatic corner override Tapping mode Cutting mode

Macro modal call Macro modal call cancel Coordinate rotation Coordinate rotation cancel

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

Peck drilling cycle

Absolute command Increment command Setting for work coordinate system or clamp at maximum spindle

speed

B–62704EN/03

G code FunctionGroup

G94 G95 G96

G97 G98 G99

3. PREP ARATORY FUNCTION

PROGRAMMING

T able 3 G code list (3/3)

Feed per minute Feed per rotation Constant surface speed control Constant surface speed control cancel Return to initial point in canned cycle Return to R point in canned cycle

(G FUNCTION)

4. INTERPOLA TION FUNCTIONS

INTERPOLATION FUNCTIONS

PROGRAMMING

B–62704EN/03

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.1 POSITIONING (G00)

Format

Explanations

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

G00 _;IP

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

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

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

D Nonlinear interpolation positioning

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

D Linear interpolation positioning

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

Start position

Linear interpolation positioning

End position

Non linear interpolation positioning

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

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62704EN/03

Limitations

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

D G28 specifying positioning between the reference and intermediate

positions.

D G53

B–62704EN/03

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.2 SINGLE DIRECTION POSITIONING (G60)

Format

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

Overrun

Start position

End position

G60 _;

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

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

Temporary stop

Explanations

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

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

Example)

When one–shot G60 commands are used.

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

Single direction positioning

When modal G60 command is used.

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

Single direction positioning mode start

Single direction positioning

Dwell Single direction

positioning mode cancel

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62704EN/03

Restrictions

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

effected in Z axis.

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

overrun has been set by the parameter.

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

positioning is not performed.

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

the canned cycles of G76 and G87.

B–62704EN/03

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.3

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 commnad, the distance the tool moves.

F_:Speed of tool feed (Feedrate)

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

G01ααββγγζζ

Feed rate of α axis direction :

Feed rate of β axis direction :

Feed rate of γ axis direction :

Feed rate of ζ axis direction :

L + a

Ff ;

) b2) g2) z

Fa +

Fb+

Fg +

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

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

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62704EN/03

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

Examples

D Linear interpolation

202) 40

The feed rate for the C axis is

300

0.14907

0.14907 (min)8

268.3 degńmin

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

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

Y axis

100.0

(End position)

D Feedrate for the

rotation axis

(Start position)

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

(End point)

200.00

(Start point)

90°

Feedrate is 300 deg/min

X axis

B–62704EN/03

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.4

CIRCULAR INTERPOLATION (G02,G03)

Format

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

Arc in the XpYp plane

G17

Arc in the ZpXp plane

G18

Arc in the YpZp plane

G19

G02 G03

Xp_Yp_

Xp_ Zp_

Yp_ Zp_

I_ J_ R_

I_ K_ R_

J_ K_

F_ ;

T able 4.4 Description of the command format

Command

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

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

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

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

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

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

with sign

Description

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

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

4. INTERPOLA TION FUNCTIONS

Explanations

PROGRAMMING

B–62704EN/03

D Direction of the circular

interpolation

D Distance moved on an

arc

D Distance from the start

point to the center of arc

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

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

pXp

in the positive–to–negative direction of the Z

axis (Yp axis or Xp axis,

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

Yp Xp Zp

G18

G03

G02

G19

G02

G17

G03

G02

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

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

End point (x,y)

Center

Start point

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

End point (z,x)

Center

Start point

End point (y ,z)

Center

are omitted (the end

Start point

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

B–62704EN/03

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

D Arc radius

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

For arc (1)(less than 180°)

G91 G02 X

For arc (2)(greater than 180°)

G91 G02 X

60.0 YP20.0 R50.0 F300.0 ;

60.0 YP20.0 R–50.0 F300.0 ;

r=50mm

Start point

End point

r=50mm

D Feedrate

Restrictions

D Simultaneously

command with I, J, K, and R

D If an axis not comprising

the specified plane is commanded

D Radius specification of

half-circle

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

If I, J, K, and R addresses are specified simultaneously, the arc specified by address R takes precedence and the other are ignored.

If an axis not comprising the specified plane is commanded, an alarm is displayed. For example, if axis U is specified as a parallel axis to X axis when plane XY is specified, an P/S alarm (No.028)is displayed.

When an arc having a center angle approaching 180° is specified, the calculated center coordinates may contain an error. In such a case, specify the center of the arc with I, J, and K.

4. INTERPOLA TION FUNCTIONS

Examples

PROGRAMMING

Y axis

100

B–62704EN/03

50R

140

60R

200

60 40

90 120

The above tool path can be programmed as follows ;

   

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

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

   

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

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

X axis

B–62704EN/03

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.5

HELICAL INTERPOLATION (G02,G03)

Format

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

Synchronously with arc of XpYp plane

G17

Synchronously with arc of ZpXp plane

G18

Synchronously with arc of YpZp plane

G19

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

G02 G03

Up to two other axes can be specified.

XpYp

XpZp

YpZp

IJ R_

IK



JK R

α(β)F

αβ)F_;

αβ)F;

Explanations

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

Length of linear axis

F×

Length of circular arc

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

Tool path

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

Restrictions

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

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62704EN/03

4.6

CYLINDRICAL INTERPOLATION (G07.1)

Format

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

G07.1 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.

IP IP

Explanations

D Plane selection

(G17, G18, G19)

D 

D Circular interpolation

(G02,G03)

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

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

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

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

G18 Z__C__;

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

G19 C__Z__;

G02 (G03) Z__C__R__;

B–62704EN/03

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

D Tool offset

D Cylindrical interpolation

accuracy

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

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

The actual amount of travel

MOTION REV

2×2πR

The amount of travel per rotation of the rotation axis

(360°)

Workpiece radius



Specified value

2×2πR



MOTION REV

Limitations

D Arc radius specification

in the cylindrical interpolation mode

D Circular interpolation

and cutter compensation

D Positioning

D Coordinate system

setting

D Cylindrical interpolation

mode setting

Rounded to the least input increment

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

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

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

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

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

D Tool offset

D Index table indexing

function

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

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

4. INTERPOLA TION FUNCTIONS

Examples

PROGRAMMING

B–62704EN/03

Example of a Cylindrical Interpolation Program

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

120 110

70 60

N05

N06

N11

N07

N08 N09 N10

60 70

150

N12

230190

270

N13

360

deg

B–62704EN/03

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.7

THREAD CUTTING (G33)

Format

Explanations

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

G33 _ F_ ; F : Long axis direction lead



In general, thread cutting is repeated along the same tool path in rough cutting through finish cutting for a screw . Since thread cutting starts when the position coder mounted on the spindle outputs a 1–turn signal, threading is started at a fixed point and the tool path on the workpiece is unchanged for repeated thread cutting. Note that the spindle speed must remain constant from rough cutting through finish cutting. If not, incorrect thread lead will occur. In general, the lag of the servo system, etc. will produce somewhat incorrect leads at the starting and ending points of a thread cut. To compensate for this, a thread cutting length somewhat longer than required should be specified. Table 4.7 lists the ranges for specifying the thread lead.

T able. 4.7 Ranges of lead sizes that can be specified

mm inpu

Least command

increment

0.001 mm F1 to F50000 (0.01 to 500.00mm)

0.0001 mm F1 to F50000 (0.01 to 500.00mm)

0.0001 inch F1 to F99999 (0.0001 to 9.9999inch)

Command value range of the lead

Inch input

0.00001 inch F1 to F99999 (0.0001 to 9.9999inch)

4. INTERPOLA TION FUNCTIONS

NOTE

1 The spindle speed is limited as follows :

PROGRAMMING

B–62704EN/03

1  spindle speed 

Maximum feedrate

Thread lead

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

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

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

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

is terminated)

Examples

Thread cutting at a pitch of 1.5mm

G33 Z10. F1.5;

B–62704EN/03

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.8

SKIP FUNCTION(G31)

Format

Explanations

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

G31 _ ;

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

is specified)

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

#5061 1st axis coordinate value #5062 2nd axis coordinate value #5063 3rd axis coordinate value #5064 4th axis coordinate value

WARNING

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

NOTE

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

4. INTERPOLA TION FUNCTIONS

Examples D The next block to G31 is

an incremental command

PROGRAMMING

G31 G91X100.0 F100;

Y50.0;

B–62704EN/03

D The next block to G31 is

an absolute command for 1 axis

Skip signal is input here

Fig. 4.8 (a) The next block is an incremental command

G31 G90X200.00 F100;

Y100.0;

Skip signal is input here

100.0

50.0

Actual motion Motion without skip signal

Y100.0

X200.0

D The next block to G31 is

an absolute command for 2 axes

Actual motion Motion without skip signal

Fig. 4.8 (b) The next block is an absolute command for 1 axis

G31 G90X200.0 F100;

X300.0 Y100.0; Y

Skip signal is input here

100

100 200 300

Fig. 4.8 (c) The next block is an absolute command for 2 axes

(300,100)

Actual motion Motion without skip signal

B–62704EN/03

 

PROGRAMMING

5. FEED FUNCTIONS

PROGRAMMING

B–62704EN/03

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

Feed rate

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

: Feedrate

: Acceleration/

Time

deceleration time constant for a cutting feedrate

Time

B–62704EN/03

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)).

Fig. 5.1 (c) Example of radial error in circular interpolation

∆r:Error

Programmed path Actual tool path

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 IP_ ;

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

B–62704EN/03

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–62704EN/03

PROGRAMMING

5. FEED FUNCTIONS

5.3

CUTTING FEED

Format

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. Four modes of specification are available:

1. Feed per minute (G94) After F, specify the amount of feed of the tool per minute.

2. Feed per revolution (G95) After F, specify the amount of feed of the tool per spindle revolution.

3. Inverse time feed (G93) Specify the inverse time (FRN) after F.

4. F1–digit feed Specify a desired one–digit number after F . Then, the feedrate set with the CNC for that number is set.

Feed per minute

G94 ; G code (group 05) for feed per minute F_ ; Feedrate command (mm/min or inch/min)

Feed per revolution

G95 ; G code (group 05) for feed per revolution F_ ; Feedrate command (mm/rev or inch/rev)

Explanations

D Tangential speed

constant control

Inverse time feed (G93)

G93 ; Inverse time feed command

G code (05 group)

F_ ; Feedrate command (1/min)

F1–digit feed

Fn ; n : Number from 1 to 9

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

End point

Start point

Linear interpolation

Starting point

Center

Circular interpolation

End point

Fig. 5.3 (a) Tangential feedrate (F)

5. FEED FUNCTIONS

PROGRAMMING

B–62704EN/03

D Feed per minute (G94)

After specifying G94 (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 . G94 is a modal code. Once a G94 is specified, it is valid until G95 (feed per revolution) is specified. At power–on, the feed per minute 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.

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

Tool

Workpiece

Table

Fig. 5.3 (b) Feed per minute

WARNING

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

D Feed per revolution

(G95)

After specifying G95 (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 . G95 is a modal code. Once a G95 is specified, it is valid until G94 (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.

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

Fig. 5.3 (c) Feed per revolution

CAUTION

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

B–62704EN/03

PROGRAMMING

5. FEED FUNCTIONS

D One–digit F code feed

D Cutting feedrate clamp

When a one–digit number from 1 to 9 is specified after F, the feedrate set for that number in a parameter (Nos. 1451 to 1459) is used. When F0 is specified, the rapid traverse rate is applied. The feedrate corresponding to the number currently selected can be increased or decreased by turning on the switch for changing F1–digit feedrate on the machine operator’s panel, then by rotating the manual pulse generator. The increment/decrement, ∆F, in feedrate per scale of the manual pulse generator is as follows:

F 

Fmax 100X

∆

Fmax : feedrate upper limit for F1–F4 set by parameter (No.1460), or

feedrate upper limit for F5–F9 set by parameter (No.1461)

X :any value of 1–127 set by parameter (No.1450) The feedrate set or altered is kept even while the power is off. The current feed rate is displayed on the CRT screen.

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. Parameter No. 1430 can be used to specify the maximum cutting feedrate for each axis only for linear interpolation and circular interpolation. When the cutting feedrate along an axis exceeds the maximum feedrate for the axis as a result of interpolation, the cutting feedrate is clamped to the maximum feedrate.

Reference

NOTE

An upper limit is set in mm/min or inch/min. CNC calculation may involve a feedrate error of ±2% with respect to a specified value. However, this is not true for acceleration/deceleration. To be more specific, this error is calculated with respect to a measurement on the time the tool takes to move 500 mm or more during the steady state:

See Appendix C for range of feedrate command value.

5. FEED FUNCTIONS

–

PROGRAMMING

B–62704EN/03

5.4

CUTTING FEEDRATE CONTROL

Function name

Exact stop G09

Exact stop mode G61

Cutting mode G64

Tapping mode G63

Auto mati

Automatic override for inner corners

G code Validity of G code Description

G62

Cutting feedrate can be controlled, as indicated in Table 5.4.

Table 5.4 Cutting Feedrate Control

This function is valid for specified blocks only.

Once specified, this function is valid until G62, G63, or G64 is specified.

Once specified, this function is valid until G61, G62, or G63 is specified.

Once specified, this function is valid until G61, G62, or G64 is specified.

Once specified, this function is valid until G61, G63, or G64 is specified.

The tool is decelerated at the end point of a block, then an in–position check is made. Then the next block is executed.

The tool is not decelerated at the end point of a block, but the next block is executed.

The tool is not decelerated at the end point of a block, but the next block is executed. When G63 is specified, feedrate override and feed hold are invalid.

When the tool moves along an inner corner during cutter compensation, override is applied to the cutting feedrate to suppress the amount of cutting per unit of time so that a good surface finish can be produced.

Internal circular cutting feedrate change

This function is valid in the cutter compensation mode, regardless of

the G code.

NOTE

1 The purpose of in–position check is to check that the servo

motor has reached within a specified range (specified with a parameter by the machine tool builder). In–position check is not performed when bit 5 (NCI) of parameter No. 1601 is set to 1.

2 Inner corner angle θ: 2°

(α is a set value)

The internal circular cutting feedrate is changed.

< θ  α  178°

Workpiece

Tool

B–62704EN/03

Format

PROGRAMMING

5. FEED FUNCTIONS

5.4.1

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

Explanations

Exact stop G09 IP_ ; Exact stop mode G61 ;

Cutting mode G64 ; Tapping mode G63 ; Automatic corner override G62 ;

The inter–block paths followed by the tool in the exact stop mode, cutting mode, and tapping mode are different (Fig. 5.4.1).

(2)

(1)

In–position check Tool path in the exact stop mode

Tool path in the cutting mode or tapping mode

Fig. 5.4.1 Example of tool paths from block (1) to block (2)

CAUTION

The cutting mode (G64 mode) is set at power–on or system clear.

5. FEED FUNCTIONS

PROGRAMMING

B–62704EN/03

5.4.2

Automatic Corner Override

When cutter compensation is performed, the movement of the tool is automatically decelerated at an inner corner and internal circular area. This reduces the load on the cutter and produces a smoothly machined surface.

5.4.2.1

Automatic Override for Inner Corners (G62)

Explanations

D Override condition

1. Straight line–straight line 2. Straight line–arc

When G62 is specified, and the tool path with cutter compensation applied forms an inner corner, the feedrate is automatically overridden at both ends of the corner. There are four types of inner corners (Fig. 5.4.2.1 (a)). 2,

θθp178, in Fig. 5.4.2.1 (a) θp is a value set with parameter No. 1711. When θ is approximately

equal to

θp, the inner corner is determined with an error of 0.001,or

less.

Tool Programmed path Cutter center path

3. Arc–straight line 4. Arc–arc

Fig. 5.4.2.1 (a) Inner corner

B–62704EN/03

PROGRAMMING

5. FEED FUNCTIONS

Override range

When a corner is determined to be an inner corner, the feedrate is overridden before and after the inner corner. The distances Ls and Le, where the feedrate is overridden, are distances from points on the cutter center path to the corner (Fig. 5.4.2.1 (b), Fig. 5.4.2.1 (c), Fig. 5.4.2.1 (d)). Ls and Le are set with parameter Nos. 1713 and 1714.

Programmed path

Cutter center path

The feedrate is overridden from point a to point b.

FIg. 5.4.2.1 (b) Override Range (Straight Line to Straight Line)

When a programmed path consists of two arcs, the feedrate is overridden if the start and end points are in the same quadrant or in adjacent quadrants (Fig. 5.4.2.1 (c)).

Cutter center path

The feedrate is overridden from point a to b.

Fig. 5.4.2.1 (c) Override Range (Arc to Arc)

Programmed path

5. FEED FUNCTIONS

PROGRAMMING

B–62704EN/03

Regarding program (2) of an arc, the feedrate is overridden from point a to point b and from point c to point d (Fig. 5.4.2.1 (d)).

Programmed path

d a

LsLebLs Le

(2)

Override value

Limitations

D Acceleration/decelera-

tion before interpolation

D Start–up/G41, G42

D Offset

Tool

Cutter center path

Fig. 5.4.2.1 (d) Override Range (Straight Line to Arc, Arc to Straight Line)

An override value is set with parameter No. 1712. An override value is valid even for dry run and F1–digit specification. In the feed per minute mode, the actual feedrate is as follows:

F × (automatic override for inner corners) × (feedrate override)

Override for inner corners is disabled during acceleration/deceleration before interpolation.

Override for inner corners is disabled if the corner is preceded by a start–up block or followed by a block including G41 or G42.

Override for inner corners is not performed if the offset is zero.

B–62704EN/03

PROGRAMMING

5. FEED FUNCTIONS

5.4.2.2

Internal Circular Cutting Feedrate Change

For internally offset circular cutting, the feedrate on a programmed path is set to a specified feedrate (F) by specifying the circular cutting feedrate with respect to F , as indicated below (Fig. 5.4.2.2). This function is valid in the cutter compensation mode, regardless of the G62 code.

Rc : Cutter center path radius Rp : Programmed radius

It is also valid for the dry run and the one–digit F command.

Programmed path

Cutter center

Fig. 5.4.2.2 Internal circular cutting feedrate change

path

If Rc is much smaller than Rp, Rc/Rp80; the tool stops. A minimum deceleration ratio (MDR) is to be specified with parameter No. 1710. When Rc/Rp

xMDR, the feedrate of the tool is (F×MDR).

NOTE

When internal circular cutting must be performed together with override for inner corners, the feedrate of the tool is as follows:

(override for the inner corners)

×(feedrate override)

5. FEED FUNCTIONS

s or rev

5.5

DWELL (G04)

Format

PROGRAMMING

Dwell G04 X_ ; or G04 P_ ;

X_ : Specify a time or spindle speed (decimal point permitted) P_ : Specify a time or spindle speed (decimal point not permitted)

B–62704EN/03

Explanations

By specifying a dwell, the execution of the next block is delayed by the specified time. In addition, a dwell can be specified to make an exact check in the cutting mode (G64 mode). When neither P nor X is specified, exact stop is performed. Bit 1 (DWL) of parameter No. 3405 can specify dwell for each rotation in feed per rotation mode (G95).

T able 5.5 (a) Command value range of the dwell time

(Command by X)

Increment system

IS–B IS–C

T able 5.5 (b) Command value range of the dwell time

Increment system

IS–B 1 to 99999999 0.001 s or rev. IS–C 1 to 99999999 0.0001 s or rev .

Command value range Dwell time unit

0.001 to 99999.999 .

0.0001 to 9999.9999

(Command by P)

Command value range Dwell time unit

B–62704EN/03

PROGRAMMING

REFERENCE POSITION

A CNC machine tool has a special position where, generally, the tool is exchanged or the coordinate system is set, as described later. This position is referred to as a reference position.

6. REFERENCE POSITION

6.1 REFERENCE POSITION RETURN

General

PROGRAMMING

B–62704EN/03

D Reference position

The reference position is a fixed position on a machine tool to which the tool can easily be moved by the reference position return function. For example, the reference position is used as a position at which tools are automatically changed. Up to four reference positions can be specified by setting coordinates in the machine coordinate system in parameters (No. 1240 to 1243).

2nd reference position

3rd reference position

Reference position

4th reference position

Machine zero point

Fig. 6.1 (a) Machine zero point and reference positions

B–62704EN/03

PROGRAMMING

6. REFERENCE POSITION

D Reference position

return and movement from the reference position

Tools are automatically moved to the reference position via an intermediate position along a specified axis. Or, tools are automatically moved from the reference position to a specified position via an intermediate position along a specified axis. When reference position return is completed, the lamp for indicating the completion of return goes on.

Reference position returnA→B→R Return from the reference positionR→B→C

B (Intermediate position)

A (Start position for reference position return)

Fig. 6.1 (b) Reference position return and return from the reference

C (Destination of return from the reference position)

position

R (Reference position)

D Reference position

return check

Format

D Reference position

return

D Return from reference

position

The reference position return check (G27) is the function which checks whether the tool has correctly returned to the reference position as specified in the program. If the tool has correctly returned to the reference position along a specified axis, the lamp for the axis goes on.

G28 _ ;

G30 P2 _ ;

G30 P3 _ ;

G30 P4 _ ;

: Command specifying the intermediate position

(Absolute/incremental command)

G29 _ ;

Reference position return

2nd reference position return

3rd reference position return

4th reference position return

(P2 can be omitted.)

: Command specifying the destination of return from reference

position (Absolute/incremental command)

D Reference position

return check

G27 _ ;

: Command specifying the reference position

(Absolute/incremental command)

6. REFERENCE POSITION



PROGRAMMING

B–62704EN/03

D Reference position

return (G28)

D 2nd, 3rd, and 4th

reference position return (G30)

D Return from the

reference position (G29)

Positioning to the intermediate or reference positions are performed at the rapid traverse rate of each axis. Therefore, for safety, the cutter compensation, and tool length compensation should be cancelled before executing this command. The coordinates for the intermediate position are stored in the CNC only for the axes for which a value is specified in a G28 block. For the other axes, the previously specified coordinates are used.

Example N1 G28 X40.0 ; Intermediate position (X40.0)

N2 G28 Y60.0 ; Intermediate position (X40.0, Y60.0)

In a system without an absolute–position detector, the second, third, and fourth reference position return functions can be used only after the first reference position return (G28) or manual reference position return (see III–3.1) is made. The G30 command is generally used when the automatic tool changer (ATC) position differs from the reference position.

In general, it is commanded immediately following the G28 command or G30. For incremental programming, the command value specifies the incremental value from the intermediate point. Positioning to the intermediate or reference points are performed at the rapid traverse rate of each axis. When the workpiece coordinate system is changed after the tool reaches the reference position through the intermediate point by the G28 command, the intermediate point also shifts to a new coordinate system. If G29 is then commanded, the tool moves to to the commanded position through the intermediate point which has been shifted to the new coordinate system. The same operations are performed also for G30 commands.

D Reference position

return check (G27)

Restrictions D Status the machine lock

being turned on

D First return to the

reference position after the power has been turned on (without an absolute position detector)

G27 command positions the tool at rapid traverse rate. If the tool reaches the reference position, the reference position return lamp lights up. If a return to the reference position of only one axis is completed, a lamp only corresponding to that axis goes on. However, if the position reached by the tool is not the reference position after positioning, an alarm (No. 092) is displayed.

The lamp for indicating the completion of return does not go on when the machine lock is turned on, even when the tool has automatically returned to the reference position. In this case, it is not checked whether the tool has returned to the reference position even when a G27 command is specified.

When the G28 command is specified when manual return to the reference position has not been performed after the power has been turned on, the movement from the intermediate point is the same as in manual return to the reference position. In this case, the tool moves in the direction for reference position return specified in parameter ZMIx (bit 5 of No. 1006). Therefore the specified intermediate position must be a position to which reference position return is possible.

B–62704EN/03

PROGRAMMING

6. REFERENCE POSITION

D Reference position

return check in an offset mode

D Lighting the lamp when

the programmed position does not coincide with the reference position



D Manual reference

position return

Examples

In an offset mode, the position to be reached by the tool with the G27 command is the position obtained by adding the offset value. Therefore, if the position with the offset value added is not the reference position, the lamp does not light up, but an alarm is displayed instead. Usually , cancel offsets before G27 is commanded.

When the machine tool system is an inch system with metric input, the reference position return lamp may also light up even if the programmed position is shifted from the reference position by the least setting increment. This is because the least setting increment of the machine tool system is smaller than its least command increment.

See III–3.1.

G28G90X1000.0Y500.0 ; (Programs movement from A to B) T1111 ; (Changing the tool at the reference position) G29X1300.0Y200.0 ; (Programs movement from B to C)

The tool is changed at the reference position

Reference position

500

300 200

Fig. 6.1 (c) Reference position return and return from the reference

200 1000 1300

position

7. COORDINA TE SYSTEM

COORDINATE SYSTEM

PROGRAMMING

By teaching the CNC a desired tool position, the tool can be moved to the position. Such a tool position is represented by coordinates in a coordinate system. Coordinates are specified using program axes. When three program axes, the X–axis, Y–axis, and Z–axis, are used, coordinates are specified as follows:

X_Y_Z_

This command is referred to as a dimension word.

B–62704EN/03

25.0

50.0

40.0

Fig. 7 Tool position specified by X40.0Y50.0Z25.0

Coordinates are specified in one of following three coordinate systems: (1)Machine coordinate system (2)Workpiece coordinate system (3)Local coordinate system

The number of the axes of a coordinate system varies from one machine to another. So, in this manual, a dimension word is represented as IP_.

B–62704EN/03

PROGRAMMING

7. COORDINA TE SYSTEM

7.1

MACHINE COORDINATE SYSTEM

Format

Explanations

D Selecting a machine

coordinate system (G53)

The point that is specific to a machine and serves as the reference of the machine is referred to as the machine zero point. A machine tool builder sets a machine zero point for each machine. A coordinate system with a machine zero point set as its origin is referred to as a machine coordinate system. A machine coordinate system is set by performing manual reference position return after power–on (see III–3.1). A machine coordinate system, once set, remains unchanged until the power is turned off.

(G90)G53 IP _ ;

IP _; Absolute dimension word

When a command is specified the position on a machine coordinate system, the tool moves to the position by rapid traverse. G53, which is used to select a machine coordinate system, is a one–shot G code; that is, it is valid only in the block in which it is specified on a machine coordinate system. Specify an absolute command (G90) for G53. When an incremental command (G91) is specified, the G53 command is ignored. When the tool is to be moved to a machine–specific position such as a tool change position, program the movement in a machine coordinate system based on G53.

Restrictions

D Cancel of the

compensation function

D G53 specification

immediately after power–on

Reference

When the G53 command is specified, cancel the cutter compensation, tool length offset, and tool offset.

Since the machine coordinate system must be set before the G53 command is specified, at least one manual reference position return or automatic reference position return by the G28 command must be performed after the power is turned on. This is not necessary when an absolute–position detector is attached.

When manual reference position return is performed after power–on, a machine coordinate system is set so that the reference position is at the coordinate values of (

Machine zero

α, β) set using parameter No.1240.

Machine coordinate system

Reference position

7. COORDINA TE SYSTEM

PROGRAMMING

B–62704EN/03

7.2

WORKPIECE COORDINATE SYSTEM

7.2.1

Setting a Workpiece Coordinate System

A coordinate system used for machining a workpiece is referred to as a workpiece coordinate system. A workpiece coordinate system is to be set with the CNC beforehand (setting a workpiece coordinate system). A machining program sets a workpiece coordinate system (selecting a workpiece coordinate system). A set workpiece coordinate system can be changed by shifting its origin (changing a workpiece coordinate system).

A workpiece coordinate system can be set using one of three methods:

(1) Method using G92

A workpiece coordinate system is set by specifying a value after G92 in the program.

(2) Automatic setting

If bit 0 of parameter ZPR No. 1201 is set beforehand, a workpiece coordinate system is automatically set when manual reference position return is performed (see Sec. III–3.1.).

(3) Input using the CRT/MDI panel

Six workpiece coordinate systems can be set beforehand using the MDI panel (see Subsec. III–11.4.6.). When using an absolute command, establish the workpiece coordinate system in any of the above ways.

Format

D Setting a workpiece

coordinate system by G92

Explanations

A workpiece coordinate system is set so that a point on the tool, such as the tool tip, is at specified coordinates. If a coordinate system is set using G92 during tool length offset, a coordinate system in which the position before offset matches the position specified in G92 is set. Cutter compensation is cancelled temporarily with G92.

Examples

Example 1

Setting the coordinate system by the G92X25.2Z23.0; command (The tool tip is the start point for the program.)

23.0

(G90) G92 IP_

Setting the coordinate system by the G92X600.0Z1200.0; command (The base point on the tool holder is the start point for the program.)

Example 2

1200.0

Base point

If an absolute command is issued, the base point moves to the commanded position. In order to move the tool tip to the commanded position, the difference from the tool tip to the base point is compensated by tool length offset.

25.2

600.0

B–62704EN/03

PROGRAMMING

7. COORDINA TE SYSTEM

7.2.2

Selecting a Workpiece Coordinate System

Examples

The user can choose from set workpiece coordinate systems as described below. (For information about the methods of setting, see II– 7.2.1.) (1)Once a workpiece coordinate system is selected by G92 or automatic

workpiece coordinate system setting, absolute commands work with the workpiece coordinate system.

(2)Choosing from six workpiece coordinate systems set using the

CRT/MDI panel By specifying a G code from G54 to G59, one of the workpiece coordinate systems 1 to 6 can be selected.

G54 Workpiece coordinate system 1 G55 Workpiece coordinate system 2 G56 Workpiece coordinate system 3 G57 Workpiece coordinate system 4 G58 Workpiece coordinate system 5 G59 Workpiece coordinate system 6

Workpiece coordinate system 1 to 6 are established after reference position return after the power is turned on. When the power is turned on, G54 coordinate system is selected.

G90 G55 G00 X40.0 Y100.0 ;

Workpiece coordinate system 2 (G55)

100.0

40.0

In this example, positioning is made to positions (X=40.0, Y=100.0) in workpiece coordinate system 2.

Fig. 7.2.2

7. COORDINA TE SYSTEM

PROGRAMMING

B–62704EN/03

7.2.3

Changing Workpiece Coordinate System

Workpiece coordinate system 1 (G54)

ZOFS1

Machine zero point

EXOFS : External workpiece zero point offset value ZOFS1AZOFS6 : Workpiece zero point offset value

Workpiece coordinate system 2 (G55)

EXOFS

The six workpiece coordinate systems specified with G54 to G59 can be changed by changing an external workpiece zero point offset value or workpiece zero point offset value. Three methods are available to change an external workpiece zero point offset value or workpiece zero point offset value. (1) Inputting from the MDI panel (see III–11.4.6) (2) Programming by G10 or G92 (3) Using the external data input function

An external workpiece zero point offset value can be changed by input signal to CNC. Refer to machine tool builder’s manual for details

ZOFS2

Workpiece coordinate system 3 (G56)

ZOFS3

ZOFS4

ZOFS5

ZOFS6

Workpiece coordinate system 4 (G57)

Workpiece coordinate system 5 (G58)

Workpiece coordinate system 6 (G59)

Fig. 7.2.3 Changing an external workpiece zero point offset value or workpiece zero point offset value

Format

D Changing by G10

D Changing by G92

G10 L2 Pp I _;

p=0 : External workpiece zero point offset value p=1 to 6 : Workpiece zero point offset value correspond to workpiece

IP : For an absolute command (G90), workpiece zero point offset for

G92 IP _;

coordinate system 1 to 6

each axis. For an incremental command (G91), value to be added to the set workpiece zero point offset for each axis (the result of addition becomes the new workpiece zero point offset).

B–62704EN/03

Explanations

PROGRAMMING

7. COORDINA TE SYSTEM

D Changing by G10

D Changing by G92

With the G10 command, each workpiece coordinate system can be changed separately.

By specifying G92IP_;, a workpiece coordinate system (selected with a code from G54 to G59) is shifted to set a new workpiece coordinate system so that the current tool position matches the specified coordinates (

IP _).

Then, the amount of coordinate system shift is added to all the workpiece zero point offset values. This means that all the workpiece coordinate systems are shifted by the same amount.

WARNING

When a coordinate system is set with G92 after an external workpiece zero point offset value is set, the coordinate system is not affected by the external workpiece zero point offset value. When G92X100.0Z80.0; is specified, for example, the coordinate system having its current tool reference position at X = 100.0 and Z = 80.0 is set.

7. COORDINA TE SYSTEM



YY

160

100

PROGRAMMING

G54 workpiece coordinate system

Tool position

B–62704EN/03

If G92X100Y100; is commanded when the tool is positioned at (200, 160) in G54 mode, workpiece coordinate system 1 (X’ – Y’) shifted by vector A is created.

G54 Workpiece coordinate system

1200.0

X’ – Z’ : New workpiece coordinate system X – Z : Original workpiece coordinate system A : Offset value created by G92 B : Workpiece zero point offset value in theG54 C : Workpiece zero point offset value in the G55

100

Z’

600.0

100

200

New workpiece coordinate system

X

Original workpiece coordinate system

G55 Workpiece coordinate system

Z

1200.0

600.0

Suppose that a G54 workpiece coordinate system is specified. Then, a G55 workpiece coordinate system where the black circle on the tool (figure at the left) is at (600.0,12000.0) can be set with the following command if the relative relationship between the G54 workpiece coordinate system and G55 workpiece coordinate system is set correctly:G92X600.0Z1200.0;Also, suppose that pallets are loaded at two different positions. If the relative relationship of the coordinate systems of the pallets at the two positions is correctly set by handling the coordinate systems



as the G54 workpiece coordinate system and G55 workpiece coordinate system, a coordinate system shift with G92 in one pallet causes the same coordinate system shift in the other pallet. This means that workpieces on two pallets can be machined with the same program just by specifying G54 or G55.

B–62704EN/03

PROGRAMMING

7. COORDINA TE SYSTEM

7.2.4

Workpiece coordinate system preset (G92.1)

Format

Explanations

The workpiece coordinate system preset function presets a workpiece coordinate system shifted by manual intervention to the pre–shift workpiece coordinate system. The latter system is displaced from the machine zero point by a workpiece zero point offset value. There are two methods for using the workpiece coordinate system preset function. One method uses a programmed command (G92.1). The other uses MDI operations on the absolute position display screen, relative position display screen, and overall position display screen (III– 11.1.4).

G92.1 IP 0 ;

IP 0 ; Specifies axis addresses subject to the workpiece

coordinate system preset operation. Axes that are not specified are not subject to the preset operation.

When manual reference position return operation is performed in the reset state, a workpiece coordinate system is shifted by the workpiece zero point offset value from the machine coordinate system zero point. Suppose that the manual reference position return operation is performed when a workpiece coordinate system is selected with G54. In this case, a workpiece coordinate system is automatically set which has its zero point displaced from the machine zero point by the G54 workpiece zero point offset value; the distance from the zero point of the workpiece coordinate system to the reference position represents the current position in the workpiece coordinate system.

G54 workpiece coordinate system

G54 workpiece zero

point offset value

Reference position

Manual reference position return

If an absolute position detector is provided, the workpiece coordinate system automatically set at power–up has its zero point displaced from the machine zero point by the G54 workpiece zero point offset value. The machine position at the time of power–up is read from the absolute position detector and the current position in the workpiece coordinate system is set by subtracting the G54 workpiece zero point offset value from this machine position. The workpiece coordinate system set by these operations is shifted from the machine coordinate system using the commands and operations listed next page.

fanuc 21MB, 210–MB Operator’s Manual

Specifications and Main Features

Frequently Asked Questions

User Manual