fanuc 21i-TB, 210i-TB Operator’s Manual

GE Fanuc Automation
Computer Numerical Control Products
Series 21i-TB/210i-TB
Operator's Manual
GFZ-63604EN/01 June 2002
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
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.
©Copyright 2002 GE Fanuc Automation North America, Inc.
All Rights Reserved.

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
1
SAFETY PRECAUTIONS
B–63604EN/01

DEFINITION OF WARNING, CAUTION, AND NOTE

This manual includes safety precautions for protecting the user and preventing damage to the machine. Precautions are classified into W arning and Caution according to their bearing on safety. Also, supplementary information is described as a Note. Read the Warning, Caution, and Note thoroughly before attempting to use the machine.
WARNING
Applied when there is a danger of the user being injured or when there is a danger of both the user being injured and the equipment being damaged if the approved procedure is not observed.
CAUTION
Applied when there is a danger of the equipment being damaged, if the approved procedure is not observed.
NOTE
The Note is used to indicate supplementary information other than Warning and Caution.
` Read this manual carefully, and store it in a safe place.
s–2
B–63604EN/01
2
SAFETY PRECAUTIONS

GENERAL W ARNINGS AND CAUTIONS

WARNING
1. Never attempt to machine a workpiece without first checking the operation of the machine.
Before starting a production run, ensure that the machine is operating correctly by performing a trial run using, for example, the single block, feedrate override, or machine lock function or by operating the machine with neither a tool nor workpiece mounted. Failure to confirm the correct operation of the machine may result in the machine behaving unexpectedly, possibly causing damage to the workpiece and/or machine itself, or injury to the user.
2. Before operating the machine, thoroughly check the entered data.
Operating the machine with incorrectly specified data may result in the machine behaving unexpectedly , possibly causing damage to the workpiece and/or machine itself, or injury to the user.
3. Ensure that the specified feedrate is appropriate for the intended operation. Generally , for each
machine, there is a maximum allowable feedrate. The appropriate feedrate varies with the intended operation. Refer to the manual provided with the machine to determine the maximum allowable feedrate. If a machine is run at other than the correct speed, it may behave unexpectedly , possibly causing damage to the workpiece and/or machine itself, or injury to the user.
4. When using a tool compensation function, thoroughly check the direction and amount of
compensation. Operating the machine with incorrectly specified data may result in the machine behaving unexpectedly , possibly causing damage to the workpiece and/or machine itself, or injury to the user.
5. The parameters for the CNC and PMC are factory–set. Usually , there is not need to change them.
When, however, there is not alternative other than to change a parameter, ensure that you fully understand the function of the parameter before making any change. Failure to set a parameter correctly may result in the machine behaving unexpectedly , possibly causing damage to the workpiece and/or machine itself, or injury to the user.
6. Immediately after switching on the power , do not touch any of the keys on the MDI 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.
7. The operator’s manual and programming manual supplied with a CNC unit provide an overall
description of the machine’s functions, including any optional functions. Note that the optional functions will vary from one machine model to another. Therefore, some functions described in the manuals may not actually be available for a particular model. Check the specification of the machine if in doubt.
s–3
SAFETY PRECAUTIONS
B–63604EN/01
WARNING
8. Some functions may have been implemented at the request of the machine–tool builder . When
using such functions, refer to the manual supplied by the machine–tool builder for details of their use and any related cautions.
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 of f. Such data may be deleted inadvertently, however, or it may prove necessary to delete all data from nonvolatile memory as part of error recovery. T o 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–63604EN/01
3
1. Coordinate system setting
SAFETY PRECAUTIONS

W ARNINGS AND CAUTIONS RELATED TO PROGRAMMING

This section covers the major safety precautions related to programming. Before attempting to perform programming, read the supplied operators manual and programming manual carefully such that you are fully familiar with their contents.
WARNING
If a coordinate system is established incorrectly, the machine may behave unexpectedly as a result of the program issuing an otherwise valid move command. Such an unexpected operation may damage the tool, the machine itself, the workpiece, or cause injury to the user.
2. Positioning by nonlinear interpolation
When performing positioning by nonlinear interpolation (positioning by nonlinear movement between the start and end points), the tool path must be carefully confirmed before performing programming. Positioning involves rapid traverse. If the tool collides with the workpiece, it may damage the tool, the machine itself, the workpiece, or cause injury to the user.
3. Function involving a rotation axis
When programming polar coordinate interpolation or normal–direction (perpendicular) control, pay careful attention to the speed of the rotation axis. Incorrect programming may result in the rotation axis speed becoming excessively high, such that centrifugal force causes the chuck to lose its grip on the workpiece if the latter is not mounted securely. Such mishap is likely to damage the tool, the machine itself, the workpiece, or cause injury to the user.
4. Inch/metric conversion
Switching between inch and metric inputs does not convert the measurement units of data such as the workpiece origin offset, parameter, and current position. Before starting the machine, therefore, determine which measurement units are being used. Attempting to perform an operation with invalid data specified may damage the tool, the machine itself, the workpiece, or cause injury to the user.
5. Constant surface speed control
When an axis subject to constant surface speed control approaches the origin of the workpiece coordinate system, the spindle speed may become excessively high. Therefore, it is necessary to specify a maximum allowable speed. Specifying the maximum allowable speed incorrectly may damage the tool, the machine itself, the workpiece, or cause injury to the user.
s–5
SAFETY PRECAUTIONS
WARNING
6. Stroke check
After switching on the power, perform a manual reference position return as required. Stroke check is not possible before manual reference position return is performed. Note that when stroke check is disabled, an alarm is not issued even if a stroke limit is exceeded, possibly damaging the tool, the machine itself, the workpiece, or causing injury to the user.
7. Tool post interference check
A tool post interference check is performed based on the tool data specified during automatic operation. If the tool specification does not match the tool actually being used, the interference check cannot be made correctly, possibly damaging the tool or the machine itself, or causing injury to the user. After switching on the power, or after selecting a tool post manually, always start automatic operation and specify the tool number of the tool to be used.
8. Absolute/incremental mode
B–63604EN/01
If a program created with absolute values is run in incremental mode, or vice versa, the machine may behave unexpectedly.
9. Plane selection
If an incorrect plane is specified for circular interpolation, helical interpolation, or a canned cycle, the machine may behave unexpectedly. Refer to the descriptions of the respective functions for details.
10.Torque limit skip
Before attempting a torque limit skip, apply the torque limit. If a torque limit skip is specified without the torque limit actually being applied, a move command will be executed without performing a skip.
11. Programmable mirror image
Note that programmed operations vary considerably when a programmable mirror image is enabled.
12.Compensation function
If a command based on the machine coordinate system or a reference position return command is issued in compensation function mode, compensation is temporarily canceled, resulting in the unexpected behavior of the machine. Before issuing any of the above commands, therefore, always cancel compensation function mode.
s–6
B–63604EN/01
4
1. Manual operation
SAFETY PRECAUTIONS

W ARNINGS 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 operators manual and programming manual carefully, such that you are fully familiar with their contents.
WARNING
When operating the machine manually , determine the current position of the tool and workpiece, and ensure that the movement axis, direction, and feedrate have been specified correctly. Incorrect operation of the machine may damage the tool, the machine itself, the workpiece, or cause injury to the operator.
2. Manual reference position return
After switching on the power, perform manual reference position return as required. If the machine is operated without first performing manual reference position return, it may behave unexpectedly . Stroke check is not possible before manual reference position return is performed. An unexpected operation of the machine may damage the tool, the machine itself, the workpiece, or cause injury to the user.
3. Manual numeric command
When issuing a manual numeric command, determine the current position of the tool and workpiece, and ensure that the movement axis, direction, and command have been specified correctly, and that the entered values are valid. Attempting to operate the machine with an invalid command specified may damage the tool, the machine itself, the workpiece, or cause injury to the operator.
4. Manual handle feed
In manual handle feed, rotating the handle with a large scale factor, such as 100, applied causes the tool and table to move rapidly. Careless handling may damage the tool and/or machine, or cause injury to the user.
5. Disabled override
If override is disabled (according to the specification in a macro variable) during threading, rigid tapping, or other tapping, the speed cannot be predicted, possibly damaging the tool, the machine itself, the workpiece, or causing injury to the operator.
6. Origin/preset operation
Basically, never attempt an origin/preset operation when the machine is operating under the control of a program. Otherwise, the machine may behave unexpectedly, possibly damaging the tool, the machine itself, the tool, or causing injury to the user.
s–7
SAFETY PRECAUTIONS
WARNING
7. Workpiece coordinate system shift
Manual intervention, machine lock, or mirror imaging may shift the workpiece coordinate system. Before attempting to operate the machine under the control of a program, confirm the coordinate system carefully. If the machine is operated under the control of a program without making allowances for any shift in the workpiece coordinate system, the machine may behave unexpectedly, possibly damaging the tool, the machine itself, the workpiece, or causing injury to the operator.
8. Software operator ’s panel and menu switches
Using the software operators panel and menu switches, in combination with the MDI panel, it is possible to specify operations not supported by the machine operators 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–63604EN/01
9. 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–63604EN/01
5
1. Memory backup battery replacement
SAFETY PRECAUTIONS

W ARNINGS RELATED TO DAILY MAINTENANCE

WARNING
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 operators panel or screen. When a low battery voltage alarm is displayed, replace the batteries within a week. Otherwise, the contents of the CNCs memory will be lost. Refer to the maintenance section of the operators manual or programming manual for details of the battery replacement procedure.
s–9
SAFETY PRECAUTIONS
B–63604EN/01
WARNING
2. Absolute pulse coder 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.
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 operators 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 operators manual or programming manual for details of the battery replacement procedure.
and
s–10
B–63604EN/01
3. Fuse replacement
SAFETY PRECAUTIONS
WARNING
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–63604EN/01

Table of Contents

SAFETY PRECAUTIONS s–1. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
I. GENERAL
1. GENERAL 3. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.1 GENERAL FLOW OF OPERATION OF CNC MACHINE TOOL 6. . . . . . . . . . . . . . . . . . . . . . . . .
1.2 CAUTIONS ON READING THIS MANUAL 8. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.3 CAUTIONS ON VARIOUS KINDS OF DATA 8. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
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 T ool – Absolute,
1.4 CUTTING SPEED – SPINDLE SPEED FUNCTION 21. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.5 SELECTION OF TOOL USED FOR VARIOUS MACHINING – TOOL FUNCTION 22. . . . . . . . . .
1.6 COMMAND FOR MACHINE OPERATIONS – MISCELLANEOUS FUNCTION 22. . . . . . . . . . . .
1.7 PROGRAM CONFIGURATION 23. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.8 COMPENSATION FUNCTION 26. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.9 TOOL MOVEMENT RANGE – STROKE 27. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
CNC – Coordinate System 16. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Incremental Commands 19. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2. CONTROLLED AXES 28. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.1 CONTROLLED AXES 29. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.2 NAMES OF AXES 29. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.3 INCREMENT SYSTEM 30. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.4 MAXIMUM STROKES 31. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3. PREPARATORY FUNCTION (G FUNCTION) 32. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4. INTERPOLATION FUNCTIONS 37. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.1 POSITIONING (G00) 38. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.2 LINEAR INTERPOLATION (G01) 40. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.3 CIRCULAR INTERPOLATION (G02, G03) 41. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.4 POLAR COORDINATE INTERPOLATION (G12.1, G13.1) 45. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.5 CYLINDRICAL INTERPOLATION (G07.1) 49. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.6 CONSTANT LEAD THREADING (G32) 53. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.7 VARIABLE–LEAD THREAD CUTTING (G34) 57. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.8 CONTINUOUS THREAD CUTTING 58. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.9 MULTIPLE–THREAD CUTTING 59. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.10 SKIP FUNCTION (G31) 61. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
c–1
Table of Contents
4.11 MULTISTAGE SKIP 63. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.12 TORQUE LIMIT SKIP (G31 P99) 64. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
B–63604EN/02
5. FEED FUNCTIONS 66. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.1 GENERAL 67. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.2 RAPID TRAVERSE 68. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.3 CUTTING FEED 69. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.4 DWELL (G04) 71. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
6. REFERENCE POSITION 72. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
6.1 REFERENCE POSITION RETURN 73. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7. COORDINATE SYSTEM 76. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.1 MACHINE COORDINATE SYSTEM 77. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.2 WORKPIECE COORDINATE SYSTEM 78. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.2.1 Setting a Workpiece Coordinate System 78. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.2.2 Selecting a W orkpiece Coordinate System 80. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.2.3 Changing Workpiece Coordinate System 81. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.2.4 W orkpiece Coordinate System Preset (G92.1) 83. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.2.5 W orkpiece Coordinate System Shift 85. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.3 LOCAL COORDINATE SYSTEM 86. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.4 PLANE SELECTION 88. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8. COORDINATE VALUE AND DIMENSION 89. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.1 ABSOLUTE AND INCREMENTAL PROGRAMMING (G90, G91) 90. . . . . . . . . . . . . . . . . . . . . . .
8.2 INCH/METRIC CONVERSION (G20, G21) 91. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3 DECIMAL POINT PROGRAMMING 92. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.4 DIAMETER AND RADIUS PROGRAMMING 93. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9. SPINDLE SPEED FUNCTION 94. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.1 SPECIFYING THE SPINDLE SPEED WITH A CODE 95. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.2 SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY (S5–DIGIT COMMAND) 95. . . . . . . . .
9.3 CONSTANT SURFACE SPEED CONTROL (G96, G97) 96. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4 SPINDLE SPEED FLUCTUATION DETECTION FUNCTION (G25, G26) 100. . . . . . . . . . . . . . . . .
9.5 SPINDLE POSITIONING FUNCTION 103. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.5.1 Spindle Orientation 103. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.5.2 Spindle Positioning 103. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.5.3 Canceling Spindle Positioning 105. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
10.TOOL FUNCTION (T FUNCTION) 106. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
10.1 TOOL SELECTION 107. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
10.2 TOOL LIFE MANAGEMENT 108. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
10.2.1 Program of Tool Life Data 108. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
10.2.2 Counting a T ool Life 111. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
10.2.3 Specifying a T ool Group in a Machining Program 112. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.AUXILIARY FUNCTION 113. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
c–2
B–63604EN/01
Table of Contents
11.1 AUXILIARY FUNCTION (M FUNCTION) 114. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.2 MULTIPLE M COMMANDS IN A SINGLE BLOCK 115. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.3 THE SECOND AUXILIARY FUNCTIONS (B CODES) 116. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
12.PROGRAM CONFIGURATION 117. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
12.1 PROGRAM COMPONENTS OTHER THAN PROGRAM SECTIONS 119. . . . . . . . . . . . . . . . . . . . .
12.2 PROGRAM SECTION CONFIGURATION 122. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
12.3 SUBPROGRAM (M98, M99) 128. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.FUNCTIONS TO SIMPLIFY PROGRAMMING 131. . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.1 CANNED CYCLE (G90, G92, G94) 132. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.1.1 Outer Diameter / Internal Diameter Cutting Cycle (G90) 132. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.1.2 Thread Cutting Cycle (G92) 134. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.1.3 End Face Turning Cycle (G94) 137. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.1.4 How to Use Canned Cycles (G90, G92, G94) 140. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.2 MULTIPLE REPETITIVE CYCLE (G70 – G76) 142. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.2.1 Stock Removal in Turning (G71) 142. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.2.2 Stock Removal in Facing (G72) 146. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.2.3 Pattern Repeating (G73) 147. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.2.4 Finishing Cycle (G70) 148. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.2.5 End Face Peck Drilling Cycle (G74) 151. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.2.6 Outer Diameter / Internal Diameter Drilling Cycle (G75) 152. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.2.7 Multiple Thread Cutting Cycle (G76) 153. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.2.8 Notes on Multiple Repetitive Cycle (G70 – G76) 158. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.3 CANNED CYCLE FOR DRILLING (G80 – G89) 159. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.3.1 Front Drilling Cycle (G83) / Side Drilling Cycle (G87) 163. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.3.2 Front Tapping Cycle (G84) / Side Tapping Cycle (G88) 166. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.3.3 Front Boring Cycle (G85) / Side Boring Cycle (G89) 168. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.3.4 Canned Cycle for Drilling Cancel (G80) 169. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.3.5 Precautions to be T aken by Operator 170. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.4 CHAMFERING AND CORNER R 171. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.5 MIRROR IMAGE FOR DOUBLE TURRET (G68, G69) 174. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.6 DIRECT DRAWING DIMENSIONS PROGRAMMING 175. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.7 RIGID TAPPING 180. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.7.1 Front Face Rigid T apping Cycle (G84) / Side Face Rigid Tapping Cycle (G88) 181. . . . . . . . . . . . . . . . . .
14.COMPENSATION FUNCTION 184. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.1 TOOL OFFSET 185. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.1.1 T ool Geometry Offset and Tool Wear Offset 185. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.1.2 T Code for T ool Offset 186. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.1.3 T ool Selection 186. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.1.4 Offset Number 186. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.1.5 Offset 187. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.1.6 G53, G28, G30, and G30.1 Commands When T ool Position Offset is Applied 190. . . . . . . . . . . . . . . . . .
14.2 OVERVIEW OF TOOL NOSE RADIUS COMPENSATION 194. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.2.1 Imaginary Tool Nose 194. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.2.2 Direction of Imaginary T ool Nose 196. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.2.3 Offset Number and Offset Value 197. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.2.4 W ork Position and Move Command 199. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.2.5 Notes on Tool Nose Radius Compensation 204. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.3 DETAILS OF TOOL NOSE RADIUS COMPENSATION 207. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
c–3
Table of Contents
14.3.1 General 207. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.3.2 T ool Movement in Start–up 209. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.3.3 T ool Movement in Of fset Mode 211. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.3.4 T ool Movement in Of fset Mode Cancel 224. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.3.5 Interference Check 227. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.3.6 Overcutting by Tool Nose Radius Compensation 232. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.3.7 Correction in Chamfering and Corner Arcs 233. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.3.8 Input Command from MDI 235. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.3.9 General Precautions for Offset Operations 236. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.3.10 G53, G28, G30, and G30.1 Commands in T ool–tip Radius Compensation Mode 237. . . . . . . . . . . . . . . .
B–63604EN/02
14.4 TOOL COMPENSATION VALUES, NUMBER OF COMPENSATION VALUES,
AND ENTERING VALUES FROM THE PROGRAM (G10) 246. . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.4.1 T ool Compensation and Number of Tool Compensation 246. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.4.2 Changing of T ool Offset Value (Programmable Data Input) (G10) 247. . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.5 AUTOMATIC TOOL OFFSET (G36, G37) 248. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.CUSTOM MACRO 251. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.1 VARIABLES 252. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.2 SYSTEM VARIABLES 256. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.3 ARITHMETIC AND LOGIC OPERATION 263. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.4 MACRO STATEMENTS AND NC STATEMENTS 268. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.5 BRANCH AND REPETITION 269. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.5.1 Unconditional Branch (GOTO Statement) 269. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.5.2 Conditional Branch (IF Statement) 270. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.5.3 Repetition (WHILE Statement) 271. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.6 MACRO CALL 274. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.6.1 Simple Call (G65) 275. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.6.2 Modal Call (G66) 279. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.6.3 Macro Call Using G Code 281. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.6.4 Macro Call Using an M Code 282. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.6.5 Subprogram Call Using an M Code 283. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.6.6 Subprogram Calls Using a T Code 284. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.6.7 Sample Program 285. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.7 PROCESSING MACRO STATEMENTS 287. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.8 REGISTERING CUSTOM MACRO PROGRAMS 289. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.9 LIMITATIONS 290. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.10 EXTERNAL OUTPUT COMMANDS 291. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.11 INTERRUPTION TYPE CUSTOM MACRO 295. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.11.1 Specification Method 296. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
15.11.2 Details of Functions 297. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
16.PROGRAMMABLE PARAMETER ENTRY (G10) 304. . . . . . . . . . . . . . . . . . . . . . . . . . .
17.MEMORY OPERATION BY SERIES 10/11 TAPE FORMAT 307. . . . . . . . . . . . . . . . . .
17.1 ADDRESSES AND SPECIFIABLE VALUE RANGE FOR SERIES 10/11 TAPE FORMAT 308. . . . .
17.2 EQUAL–LEAD THREADING 309. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
17.3 SUBPROGRAM CALLING 310. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
17.4 CANNED CYCLE 311. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
17.5 MULTIPLE REPETITIVE CANNED TURNING CYCLE 312. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
17.6 CANNED DRILLING CYCLE FORMATS 314. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
c–4
B–63604EN/01
Table of Contents
18.FUNCTIONS FOR HIGH SPEED CUTTING 318. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
18.1 REMOTE BUFFER 319. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
18.2 HIGH–SPEED REMOTE BUFFER A (G05) 320. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
18.3 DISTRIBUTION PROCESSING TERMINATION MONITORING FUNCTION
FOR THE HIGH–SPEED MACHINING COMMAND (G05) 322. . . . . . . . . . . . . . . . . . . . . . . . . . . . .
19.AXIS CONTROL FUNCTION 323. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
19.1 POLYGONAL TURNING 324. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
19.2 ROTARY AXIS ROLL–OVER 329. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
19.3 SIMPLE SYNCHRONIZATION CONTROL 330. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
19.4 B–AXIS CONTROL (G100, G101, G102, G103, G110) 332. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
19.5 ANGULAR AXIS CONTROL / ARBITRARY ANGULAR AXIS CONTROL 341. . . . . . . . . . . . . . .
20.PATTERN DATA INPUT FUNCTION 343. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
20.1 DISPLAYING THE PATTERN MENU 344. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
20.2 PATTERN DATA DISPLAY 348. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
20.3 CHARACTERS AND CODES TO BE USED
FOR THE PATTERN DATA INPUT FUNCTION 352. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
III. OPERATION
1. GENERAL 357. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.1 MANUAL OPERATION 358. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.2 TOOL MOVEMENT BY PROGRAMMING – AUTOMATIC OPERATION 360. . . . . . . . . . . . . . . . .
1.3 AUTOMATIC OPERATION 361. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.4 TESTING A PROGRAM 363. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.4.1 Check by Running the Machine 363. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.4.2 How to View the Position Display Change without Running the Machine 364. . . . . . . . . . . . . . . . . . . . . .
1.5 EDITING A PART PROGRAM 365. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.6 DISPLAYING AND SETTING DATA 366. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.7 DISPLAY 369. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.7.1 Program Display 369. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.7.2 Current Position Display 370. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.7.3 Alarm Display 370. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.7.4 Parts Count Display, Run Time Display 371. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.7.5 Graphic Display (See Section III–12) 372. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.8 DATA OUTPUT 373. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2. OPERATIONAL DEVICES 374. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.1 SETTING AND DISPLAY UNITS 375. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.1.1 7.2/8.4 LCD–Mounted T ype CNC Control Unit 376. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.1.2 9.5/10.4 LCD–Mounted T ype CNC Control Unit 376. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.1.3 Stand–Alone Type Small MDI Unit 377. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.1.4 Stand–Alone Type Standard MDI Unit 378. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.1.5 Stand–Alone T ype 61 Full–Key MDI Unit 379. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.2 EXPLANATION OF THE KEYBOARD 380. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.3 FUNCTION KEYS AND SOFT KEYS 382. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.3.1 General Screen Operations 382. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
c–5
Table of Contents
2.3.2 Function Keys 383. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.3.3 Soft Keys 384. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.3.4 Key Input and Input Buffer 400. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.3.5 W arning Messages 401. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.3.6 Soft Key Configuration 402. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
B–63604EN/02
2.4 EXTERNAL I/O DEVICES 403. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.4.1 F ANUC Handy File 405. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.5 POWER ON/OFF 406. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.5.1 Turning on the Power 406. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.5.2 Screen Displayed at Power–on 407. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
2.5.3 Power Disconnection 408. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3. MANUAL OPERATION 409. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.1 MANUAL REFERENCE POSITION RETURN 410. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.2 JOG FEED 412. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.3 INCREMENTAL FEED 414. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.4 MANUAL HANDLE FEED 415. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
3.5 MANUAL ABSOLUTE ON AND OFF 418. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4. AUT OMATIC OPERA TION 423. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.1 MEMORY OPERATION 424. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.2 MDI OPERATION 427. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.3 PROGRAM RESTART 430. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.4 SCHEDULING FUNCTION 438. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.5 SUBPROGRAM CALL FUNCTION (M198) 443. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.6 MANUAL HANDLE INTERRUPTION 445. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.7 MIRROR IMAGE 448. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.8 MANUAL INTERVENTION AND RETURN 450. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.9 DNC OPERATION 452. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.10 DNC OPERATION WITH MEMORY CARD 455. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.10.1 Specification 455. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.10.2 Operations 456. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.10.2.1 DNC operation 456. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.10.2.2 Subprogram call (M198) 457. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.10.3 LIMITATION and NOTES 458. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.10.4 PARAMETER 458. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.10.5 Connecting PCMCIA Card Attachment 459. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.10.5.1 Specification number 459. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.10.5.2 Assembling 459. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
4.10.6 Recommended Memory Card 461. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5. TEST OPERATION 462. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.1 MACHINE LOCK AND AUXILIARY FUNCTION LOCK 463. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.2 FEEDRATE OVERRIDE 465. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.3 RAPID TRAVERSE OVERRIDE 466. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.4 DRY RUN 467. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
5.5 SINGLE BLOCK 468. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
c–6
B–63604EN/01
Table of Contents
6. SAFETY FUNCTIONS 471. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
6.1 EMERGENCY STOP 472. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
6.2 OVERTRAVEL 473. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
6.3 STORED STROKE CHECK 474. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
6.4 CHUCK AND TAILSTOCK BARRIERS 478. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7. ALARM AND SELF–DIAGNOSIS FUNCTIONS 485. . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.1 ALARM DISPLAY 486. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.2 ALARM HISTORY DISPLAY 488. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
7.3 CHECKING BY SELF–DIAGNOSTIC SCREEN 489. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8. DATA INPUT/OUTPUT 492. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.1 FILES 493. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.2 FILE SEARCH 495. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.3 FILE DELETION 497. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.4 PROGRAM INPUT/OUTPUT 498. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.4.1 Inputting a Program 498. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.4.2 Outputting a Program 501. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.5 OFFSET DATA INPUT AND OUTPUT 503. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.5.1 Inputting Offset Data 503. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.5.2 Outputting Offset Data 504. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6 INPUTTING AND OUTPUTTING PARAMETERS AND PITCH ERROR
COMPENSATION DATA 505. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6.1 Inputting Parameters 505. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6.2 Outputting Parameters 506. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6.3 Inputting Pitch Error Compensation Data 507. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.6.4 Outputting Pitch Error Compensation Data 508. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.7 INPUTTING/OUTPUTTING CUSTOM MACRO COMMON VARIABLES 509. . . . . . . . . . . . . . . . .
8.7.1 Inputting Custom Macro Common Variables 509. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.7.2 Outputting Custom Macro Common Variable 510. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.8 DISPLAYING DIRECTORY OF FLOPPY DISK 511. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.8.1 Displaying the Directory 512. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.8.2 Reading Files 515. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.8.3 Outputting Programs 516. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.8.4 Deleting Files 517. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.9 OUTPUTTING A PROGRAM LIST FOR A SPECIFIED GROUP 519. . . . . . . . . . . . . . . . . . . . . . . . .
8.10 DATA INPUT/OUTPUT ON THE ALL IO SCREEN 520. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.10.1 Setting Input/Output–Related Parameters 521. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.10.2 Inputting and Outputting Programs 522. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.10.3 Inputting and Outputting Parameters 526. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.10.4 Inputting and Outputting Offset Data 528. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.10.5 Outputting Custom Macro Common Variables 530. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.10.6 Inputting and Outputting Floppy Files 531. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.10.7 Memory Card Input/Output 536. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
8.11 DATA INPUT/OUTPUT USING A MEMORY CARD 545. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9. EDITING PROGRAMS 557. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.1 INSERTING, ALTERING AND DELETING A WORD 558. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.1.1 W ord Search 559. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.1.2 Heading a Program 561. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
c–7
Table of Contents
9.1.3 Inserting a Word 562. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.1.4 Altering a W ord 563. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.1.5 Deleting a W ord 564. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
B–63604EN/02
9.2 DELETING BLOCKS 565. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.2.1 Deleting a Block 565. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.2.2 Deleting Multiple Blocks 566. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.3 PROGRAM NUMBER SEARCH 567. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.4 SEQUENCE NUMBER SEARCH 568. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.5 DELETING PROGRAMS 570. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.5.1 Deleting One Program 570. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.5.2 Deleting All Programs 570. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.5.3 Deleting More Than One Program by Specifying a Range 571. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.6 EXTENDED PART PROGRAM EDITING FUNCTION 572. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.6.1 Copying an Entire Program 573. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.6.2 Copying Part of a Program 574. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.6.3 Moving Part of a Program 575. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.6.4 Merging a Program 576. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.6.5 Supplementary Explanation for Copying, Moving and Merging 577. . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.6.6 Replacement of W ords and Addresses 579. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.7 EDITING OF CUSTOM MACROS 581. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.8 BACKGROUND EDITING 582. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
9.9 PASSWORD FUNCTION 583. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
10.CREATING PROGRAMS 585. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
10.1 CREATING PROGRAMS USING THE MDI PANEL 586. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
10.2 AUTOMATIC INSERTION OF SEQUENCE NUMBERS 587. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
10.3 CREATING PROGRAMS IN TEACH IN MODE (PLAYBACK) 589. . . . . . . . . . . . . . . . . . . . . . . . . .
1 1.SETTING AND DISPLA YING DATA 592. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.1 SCREENS DISPLAYED BY FUNCTION KEY
11.1.1 Position Display in the Workpiece Coordinate System 600. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.1.2 Position Display in the Relative Coordinate System 601. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.1.3 Overall Position Display 603. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.1.4 Presetting the W orkpiece Coordinate System 604. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.1.5 Actual Feedrate Display 605. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.1.6 Display of Run Time and Parts Count 607. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.1.7 Operating Monitor Display 608. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.2 SCREENS DISPLAYED BY FUNCTION KEY
(IN MEMORY MODE OR MDI MODE) 610. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.2.1 Program Contents Display 611. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.2.2 Current Block Display Screen 612. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.2.3 Next Block Display Screen 613. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.2.4 Program Check Screen 614. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.2.5 Program Screen for MDI Operation 616. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.2.6 Displaying the B–axis Operation State 617. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
POS
PROG
600. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.3 SCREENS DISPLAYED BY FUNCTION KEY
11.3.1 Displaying Memory Used and a List of Programs 619. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.3.2 Displaying a Program List for a Specified Group 622. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
PROG
(IN THE EDIT MODE) 618. . . . . . . . . . . . . . .
c–8
B–63604EN/01
Table of Contents
11.4 SCREENS DISPLAYED BY FUNCTION KEY
11.4.1 Setting and Displaying the Tool Offset Value 626. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.4.2 Direct Input of T ool Offset Value 629. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.4.3 Direct Input of T ool Offset Measured B 631. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.4.4 Counter Input of Offset value 633. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.4.5 Setting the Workpiece Coordinate System Shifting Amount 634. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.4.6 Y Axis Offset 636. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.4.7 Displaying and Entering Setting Data 639. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.4.8 Sequence Number Comparison and Stop 641. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.4.9 Displaying and Setting Run Time, Parts Count, and Time 643. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.4.10 Displaying and Setting the W orkpiece Origin Offset Value 645. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.4.11 Direct Input of Measured W orkpiece Origin Offsets 646. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.4.12 Displaying and Setting Custom Macro Common V ariables 648. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.4.13 Displaying and Setting the Software Operators Panel 649. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.4.14 Displaying and Setting T ool Life Management Data 651. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.4.15 Setting and Displaying B–axis T ool Compensation 654. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.5 SCREENS DISPLAYED BY FUNCTION KEY
11.5.1 Displaying and Setting Parameters 657. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.5.2 Displaying and Setting Pitch Error Compensation Data 659. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
OFFSET SETTING
SYSTEM
11.6 DISPLAYING THE PROGRAM NUMBER, SEQUENCE NUMBER, AND STATUS,
AND WARNING MESSAGES FOR DATA SETTING OR INPUT/OUTPUT OPERATION 662. . . . .
11.6.1 Displaying the Program Number and Sequence Number 662. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.6.2 Displaying the Status and W arning for Data Setting or Input/Output Operation 663. . . . . . . . . . . . . . . . . .
625. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
656. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.7 SCREENS DISPLAYED BY FUNCTION KEY
11.7.1 External Operator Message History Display 665. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
MESSAGE
11.8 CLEARING THE SCREEN 667. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.8.1 Erase CRT Screen Display 667. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
11.8.2 Automatic Erase Screen Display 668. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
12.GRAPHICS FUNCTION 669. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
12.1 GRAPHICS DISPLAY 670. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
13.HELP FUNCTION 675. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
14.SCREEN HARDCOPY 680. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
IV. MAINTENANCE
1. METHOD OF REPLACING BATTERY 685. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.1 REPLACING BATTERY FOR LCD–MOUNTED TYPE i SERIES 686. . . . . . . . . . . . . . . . . . . . . . . .
1.2 REPLACING THE BATTERY FOR STAND–ALONE TYPE i SERIES 689. . . . . . . . . . . . . . . . . . . . .
1.3 BATTERY IN THE PANEL i (3 VDC) 692. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
1.4 BATTERY FOR SEPARATE ABSOLUTE PULSE CODERS (6 VDC) 694. . . . . . . . . . . . . . . . . . . . . .
1.5 BATTERY FOR BUILT–IN ABSOLUTE PULSE CODERS (DC6V) 695. . . . . . . . . . . . . . . . . . . . . . .
665. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
APPENDIX
A. TAPE CODE LIST 703. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
c–9
Table of Contents
B–63604EN/02
B. LIST OF FUNCTIONS AND TAPE FORMAT 706. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
C. RANGE OF COMMAND VALUE 710. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
D. NOMOGRAPHS 713. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
D.1 INCORRECT THREADED LENGTH 714. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
D.2 SIMPLE CALCULATION OF INCORRECT THREAD LENGTH 716. . . . . . . . . . . . . . . . . . . . . . . . .
D.3 TOOL PATH AT CORNER 718. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
D.4 RADIUS DIRECTION ERROR AT CIRCLE CUTTING 721. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
E. STATUS WHEN TURNING POWER ON,
WHEN CLEAR AND WHEN RESET 722. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
F. CHARACTER–TO–CODES CORRESPONDENCE TABLE 724. . . . . . . . . . . . . . . . . .
G. ALARM LIST 725. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
c–10

I. GENERAL

B–63604EN/01

GENERAL

1
About this manual
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 (Table1).
III. OPERATION
Describes the manual operation and automatic operation of a machine, procedures for inputting and outputting data, and procedures for editing a program.
IV. MAINTENANCE
Describes procedures for replacing batteries.
APPENDIX
Lists tape codes, valid data ranges, and error codes.
1. GENERAL
Some functions described in this manual may not be applied to some products. For detail, refer to the DESCRIPTIONS manual (B–63522EN).
This manual does not describe parameters in detail. For details on parameters mentioned in this manual, refer to the manual for parameters (B–63610EN).
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 21i–TB 21i–TB Series 21i
FANUC Series 210i–TB 210i–TB Series 210i
3
GENERAL1. GENERAL
B–63604EN/01
Special symbols
_
D P
I
D ;
Related manuals of Series 16i/18i/21i/160i/ 180i/210i–MODEL B
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 following table lists the manuals related to Series 16i, Series 18i, Series 21i, Series 160i, Series 180i, Series 210i–MODEL B. This manual is indicated by an asterisk(*).
Manual name
DESCRIPTIONS B–63522EN CONNECTION MANUAL (HARDWARE) B–63523EN CONNECTION MANUAL (FUNCTION) B–63523EN–1 OPERA T ORS MANUAL (16i/18i/160i/180i–TB) B–63524EN OPERATORS MANUAL (16i/18i/160i/180i–MB) B–63534EN
Specification
number
OPERATORS MANUAL (21i/210i–TB) B–63604EN * OPERATORS MANUAL (21i/210i–MB) B–63614EN MAINTENANCE MANUAL B–63525EN P ARAMETER MANUAL (16i/18i/160i/180i–MODEL B) B–63530EN P ARAMETER MANUAL (21i/210i–MODEL B) B–63610EN PROGRAMMING MANUAL Macro Compiler/Macro Executor
PROGRAMMING MANUAL FAPT MACRO COMPILER (For Personal Computer)
PROGRAMMING MANUAL C Language Executor PROGRAMMING MANUAL B–62443EN–3 CAP (T series) FANUC Super CAPi T OPERATORS MANUAL B–63284EN FANUC Symbol CAPi T OPERATORS MANUAL B–63304EN MANUAL GUIDE For Lathe PROGRAMMING MANUAL B–63343EN MANUAL GUIDE For Lathe OPERA T OR’S MANUAL B–63344EN
B–61803E–1
B–66102E
CAP (M series) FANUC Super CAPi M OPERATORS MANUAL B–63294EN MANUAL GUIDE For Milling PROGRAMMING MANUAL B–63423EN MANUAL GUIDE For Milling OPERA T ORS MANUAL B–63424EN
4
B–63604EN/01
GENERAL
1. GENERAL
Related manuals of SERVO MOTOR a series
Manual name
PMC PMC Ladder Language PROGRAMMING MANUAL B–61863E PMC C Language PROGRAMMING MANUAL B–61863E–1 Network FANUC I/O Link–II CONNECTION MANUAL B–62714EN Profibus–DP Board OPERA T OR’S MANUAL B–62924EN DeviceNet Board OPERA T OR ’S MANUAL B–63404EN Ethernet Board/DA T A SERVER Board
OPERATORS MANUAL
Specification
number
B–63354EN
The following table lists the manuals related to SER VO MOT OR a series
Manual name
AC SERVO MOTOR a series DESCRIPTIONS B–65142E AC SERVO MOTOR a series PARAMETER MANUAL B–65150E
Specification
number
AC SPINDLE MOTOR a series DESCRIPTIONS B–65152E AC SPINDLE MOTOR a series PARAMETER MANUAL B–65160E SERVO AMPLIFIER a series DESCRIPTIONS B–65162E SERVO MOTOR a series MAINTENANCE MANUAL B–65165E
5
GENERAL1. GENERAL
Cutting process
B–63604EN/01
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 OPERA TION
Part program­ming
CNC
MACHINE TOOL
Before the actual programming, make the machining plan for how to machine the part. Machining plan
1. Determination of workpieces machining range
2. Method of mounting workpieces on the machine tool
3. Machining sequence in every cutting process
4. Cutting tools and cutting conditions
Decide the cutting method in every cutting process.
Cutting process
Cutting procedure
1. Cutting method : Rough Semi Finish
2. Cutting tools
3. Cutting conditions : Feedrate Cutting depth
4. Tool path
1 2 3
End face
cutting
Outer diameter
cutting
Grooving
6
B–63604EN/01
GENERAL
1. GENERAL
Grooving
Outer diameter cutting
Workpiece
End face cutting
Prepare the program of the tool path and cutting condition according to the workpiece figure, for each cutting.
7
1.2

CAUTIONS ON READING THIS MANUAL

GENERAL1. GENERAL
CAUTION
1 The function of an CNC machine tool system depends not
only on the CNC, but on the combination of the machine tool, its magnetic cabinet, the servo system, the CNC, the operators 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 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.
B–63604EN/01
1.3

CAUTIONS ON V ARIOUS KINDS OF DATA

CAUTION
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.
8

II. PROGRAMMING

B–63604EN/01
1

GENERAL

PROGRAMMING
1. GENERAL
11
PROGRAMMING1. GENERAL
B–63604EN/01
1.1
TOOL MOVEMENT ALONG WORKPIECE P ARTS 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).
X
Tool
Workpiece
Fig.1.1 (a) Tool movement along the straight line which is parallel to Z–axis
Program G01 Z...;
Z
D Tool movement along an
arc
X
Tool
Workpiece
Fig.1.1 (b) T ool movement along the taper line
X
Workpiece
Tool
Program G02X ... Z ... R ... ; or G03X ... Z ... R ... ;
Z
Program G01 X ... Z... ;
Z
Fig. 1.1 (c) T ool movement along an arc
12
B–63604EN/01
PROGRAMMING
1. GENERAL
The term interpolation refers to an operation in which the tool moves along a straight line or arc in the way described above. Symbols of the programmed commands G01, G02, ... are called the preparatory function and specify the type of interpolation conducted in the control unit.
(a) Movement along straight line
G01 Z__; X––Z––––;
Control unit
Interpolation
a) Movement
along straight line
b) Movement
along arc
Fig. 1.1 (d) Interpolation function
(b) Movement along arc
G03X––Z––;
X axis
Y axis
Tool movement
NOTE
Some machines move workpiece (spindle) instead of tools but this manual assumes that tools are moved against workpieces.
D Thread cutting
Threads can be cut by moving the tool in synchronization with spindle rotation. In a program, specify the thread cutting function by G32.
X
Workpiece
Fig. 1.1 (e) Straight thread cutting
Tool
Z
F
Program G32Z––F––;
13
PROGRAMMING1. GENERAL
B–63604EN/01
1.2
FEED– FEED FUNCTION
X
Workpiece
Fig. 1.1 (f) T aper thread cutting
Tool
Program G32X––Z––F––;
Z
F
Movement of the tool at a specified speed for cutting a workpiece is called the feed.
Chuck
Workpiece
Tool
Fig. 1.2 Feed function
Feedrates can be specified by using actual numerics. For example, the following command can be used to feed the tool 2 mm while the workpiece makes one turn :
F2.0
The function of deciding the feed rate is called the feed function (See II–5).
14
B–63604EN/01
1.3

PART DRAWING AND TOOL MOVEMENT

PROGRAMMING
1. GENERAL
1.3.1
Reference Position (Machine–Specific Position)
Explanations
A CNC machine tool is provided with a fixed position. Normally, tool change and programming of absolute zero point as described later are performed at this position. This position is called the reference position.
Tool post
Chuck
Fig. 1.3.1 Reference position
The tool can be moved to the reference position in two ways:
1. Manual reference position return (See III–3.1) Reference position return is performed by manual button operation.
Reference position
2. Automatic reference position return (See II–6) In general, manual reference position return is performed first after the power is turned on. In order to move the tool to the reference position for tool change thereafter, the function of automatic reference position return is used.
15
1.3.2
Coordinate System on Part Drawing and Coordinate System Specified by CNC – Coordinate System
PROGRAMMING1. GENERAL
X
Part drawing
B–63604EN/01
X
Program
Z
Z
Coordinate system
CNC
Command
X
Workpiece
Explanations
D Coordinate system
Z
Machine tool
Fig. 1.3.2 (a) 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. 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.
X
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
Z
16
B–63604EN/01
PROGRAMMING
1. GENERAL
The tool moves on the coordinate system specified by the CNC in accordance with the command program generated with respect to the coordinate system on the part drawing, and cuts a workpiece into a shape on the drawing. Therefore, in order to correctly cut the workpiece as specified on the drawing, the two coordinate systems must be set at the same position.
D Methods of setting the
two coordinate systems in the same position
The following method is usually used to define two coordinate systems at the same location.
1. When coordinate zero point is set at chuck face
X
Workpiece
60
40
150
Fig. 1.3.2 (c) Coordinates and dimensions on part drawing
X
40
Z
Workpiece
Z
Fig. 1.3.2 (d) Coordinate system on lathe as specified by CNC (made to coincide with the coordinate system on part drawing)
17
PROGRAMMING1. GENERAL
2. When coordinate zero point is set at work end face.
X
B–63604EN/01
Workpiece
60
100
Fig. 1.3.2 (e) Coordinates and dimensions on part drawing
Workpiece
80
30
30
Z
X
Z
Fig. 1.3.2 (f) Coordinate system on lathe as specified by CNC
(made to coincide with the coordinate system on part drawing)
18
B–63604EN/01
1.3.3
How to Indicate Command Dimensions for Moving the Tool – Absolute, Incremental Commands
PROGRAMMING
1. GENERAL
Explanations
D Absolute command
Methods of command for moving the tool can be indicated by absolute or incremental designation (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.
Tool
X
Workpiece
φ30
70
Command specifying movement from point A to point B
G90X30.0Z70.0;
B
110
A
Z
Fig. 1.3.3 (a) Absolute command
19
Coordinates of point B
PROGRAMMING1. GENERAL
B–63604EN/01
D Incremental command
Specify the distance from the previous tool position to the next tool position.
Tool
A
X
φ60
B
Z
φ30
40
Command specifying movement from point A to point B
U–30.0W–40.0
Distance and direction for movement along each axis
D Diameter programming /
radius programming
Fig. 1.3.3 (b) Incremental command
Dimensions of the X axis can be set in diameter or in radius. Diameter programming or radius programming is employed independently in each machine.
1. Diameter programming
In diameter programming, specify the diameter value indicated on the drawing as the value of the X axis.
X
B
φ30
A
Z
Workpiece
φ40
60
80
Coordinate values of points A and B A(30.0, 80.0), B(40.0, 60.0)
Fig. 1.3.3 (c) Diameter programming
20
B–63604EN/01
PROGRAMMING
1. GENERAL
2. Radius programming
In radius programming, specify the distance from the center of the workpiece, i.e. the radius value as the value of the X axis.
X
B
20
Workpiece
60
80
Coordinate values of points A and B
A(15.0, 80.0), B(20.0, 60.0)
Fig. 1.3.3 (d) Radius programming
A
15
Z
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
–1
in min
unit.
Tool
Workpiece
Fig. 1.4 Cutting speed
V: Cutting speed
v m/min
φD
N min
–1
<When a workpiece 200 mm in diameter should be machined at a cutting speed of 300 m/min. >
–1
The spindle speed is approximately 478 min
, which is obtained from
N=1000v/πD. Hence the following command is required:
S478 ;
Commands related to the spindle speed are called the spindle speed function (See II–9). The cutting speed v (m/min) can also be specified directly by the speed value. Even when the workpiece diameter is changed, the CNC changes the spindle speed so that the cutting speed remains constant. This function is called the constant surface speed control function (See II–9.3).
21
PROGRAMMING1. GENERAL
B–63604EN/01
1.5
SELECTION OF TOOL USED FOR VARIOUS MACHINING – TOOL FUNCTION
Examples
When drilling, tapping, boring, milling or the like, is performed, it is necessary to select a suitable tool. When a number is assigned to each tool and the number is specified in the program, the corresponding tool is selected.
Tool number
01
06
02 05
04
03
Fig. 1.5 T ool used for various machining
<When No.01 is assigned to a roughing tool>
When the tool is stored at location 01 of the tool post, the tool can be selected by specifying T0101. This is called the tool function (See II–10).
Tool post
1.6
COMMAND FOR MACHINE OPERATIONS – MISCELLANEOUS FUNCTION
When machining is actually started, it is necessary to rotate the spindle, and feed coolant. For this purpose, on–off operations of spindle motor and coolant valve should be controlled (See II–11).
Coolant on/off
Chuck open/close
Workpiece
Fig. 1.6 Command for machine operations
The function of specifying the on–off operations of the components of the machine is called the miscellaneous function. In general, the function is specified by an M code. For example, when M03 is specified, the spindle is rotated clockwise at the specified spindle speed.
CW spindle rotation
22
B–63604EN/01
PROGRAMMING
1. GENERAL
1.7

PROGRAM CONFIGURATION

A group of commands given to the CNC for operating the machine is called the program. By specifying the commands, the tool is moved along a straight line or an arc, or the spindle motor is turned on and off. In the program, specify the commands in the sequence of actual tool movements.
Block
Block
Tool movement sequence
Block
Program
Block
⋅ ⋅ ⋅ ⋅
Block
Fig. 1.7 (a) Program configuration
A group of commands at each step of the sequence is called the block. The program consists of a group of blocks for a series of machining. The number for discriminating each block is called the sequence number, and the number for discriminating each program is called the program number (See II–12).
23
PROGRAMMING1. GENERAL
B–63604EN/01
Explanations
D Block
The block and the program have the following configurations.
1 block
N fffff G ff Xff.f Zfff.f M ff S ff T ff ;
Sequence number
Preparatory function
Dimension word Miscel-
laneous function
Fig. 1.7 (b) Block configuration
Spindle function
Tool func­tion
End of block
A block begins with a sequence number that identifies that block and ends with an end–of–block code. This manual indicates the end–of–block code by ; (LF in the ISO code and CR in the EIA code). The contents of the dimension word depend on the preparatory function. In this manual, the portion of the dimension word may be represent as IP_.
D Program
; 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.
24
B–63604EN/01
PROGRAMMING
1. GENERAL
D Main program and
subprogram
When machining of the same pattern appears at many portions of a program, a program for the pattern is created. This is called the subprogram. On the other hand, the original program is called the main program. When a subprogram execution command appears during execution of the main program, commands of the subprogram are executed. When execution of the subprogram is finished, the sequence returns to the main program.
Main program
⋅ ⋅
M98P1001
M98P1002
M98P1001
Subprogram #1
O1001
M99
Subprogram #2
O1002
Program for hole #1
Program for hole #2
M99
25
1.8

COMPENSATION FUNCTION

Explanations
PROGRAMMING1. GENERAL
B–63604EN/01
D Machining using the end
of cutter – Tool length compensation function
Usually, several tools are used for machining one workpiece. The tools have different tool length. It is very troublesome to change the program in accordance with the tools. Therefore, the length of each tool used should be measured in advance. By setting the difference between the length of the standard tool and the length of each tool in the CNC (data display and setting : see III–11), machining can be performed without altering the program even when the tool is changed. This function is called tool length compensation.
Workpiece
Standard tool
Rough cutting tool
Fig. 1.8 Tool offset
Finishing tool
Grooving tool
Thread cutting tool
26
B–63604EN/01
PROGRAMMING
1. GENERAL
1.9
TOOL MOVEMENT RANGE – STROKE
Limit switches are installed at the ends of each axis on the machine to prevent tools from moving beyond the ends. The range in which tools can move is called the stroke. Besides the stroke limits, data in memory can be used to define an area which tools cannot enter.
Table
Motor
Limit switch
Machine zero point
Specify these distances.
Tools cannot enter this area. The area is specified by data in memory or a program.
Besides strokes defined with limit switches, the operator can define an area which the tool cannot enter using a program or data in memory . This function is called stroke check.
27
2
PROGRAMMING2. CONTROLLED AXES

CONTROLLED AXES

B–63604EN/01
28
B–63604EN/01
2.1

CONTROLLED AXES

PROGRAMMING
Item
Number of basic controlled axes 2 axes Controlled axis expansion (total) Max. 4 axes (Included in Cs axis) Number of basic simultaneously
controlled axes Simultaneously controlled axis expansion
(total)
2. CONTROLLED AXES
21i–TB
210i–TB
2 axes
Max. 4 axes
NOTE
The number of simultaneously controllable axes for manual operation (jog feed, incremental feed, or manual handle feed) is 1 or 3 (1 when bit 0 (JAX) of parameter 1002 is set to 0 and 3 when it is set to 1).
2.2

NAMES OF AXES

Limitations
D Default axis name
D Duplicate axis name
The names of two basic axes are always X and Z; the names of additional axes can be optionally selected from A, B, C, U, V, W, and Y by using parameter No.1020.
Each axis name is determined according to parameter No. 1020. If the parameter specifies 0 or anything other than the nine letters, the axis name defaults to a number from 1 to 4. When a default axis name (1 to 4) is used, the system cannot operate in MEM or MDI mode.
If the parameter specifies an axis name more than once, only the first axis to be assigned that axis name becomes operable.
NOTE
1 When G code system A is used, the letters U, V, and W
cannot be used as an axis name (hence, the maximum of six controlled axes), because these letters are used as incremental commands for X, Y, and Z. To use the letters U, V, and W as axis names, the G code system must be B or C. Likewise, letter H is used as an incremental command for C, thus incremental commands cannot be used if A or B is used as an axis name.
2 In G76 (multiple–thread cutting), the A address in a block
specifies the tool nose angle instead of a command for axis A. If C or A is used as an axis name, C or A cannot be used as an angle command for a straight line in chamfering or direct drawing dimension programming. Therefore, “,C” and “,A” should be used according to bit 4 (CCR) of parameter No.
3405.
29
PROGRAMMING2. CONTROLLED AXES
B–63604EN/01
2.3

INCREMENT SYSTEM

The increment system consists of the least input increment (for input ) and least command increment (for output). The least input increment is the least increment for programming the travel distance. The least command increment is the least increment for moving the tool on the machine. Both increments are represented in mm, inches, or degrees. The increment system is classified into IS–B and IS–C (Tables 2.3(a) and
2.3(b)). Select IS–B or IS–C using bit 1 (ISC) of parameter 1004. When
the IS–C increment system is selected, it is applied to all axes and the 1/10 increment system option is required.
T able 2.3 (a) Increment system IS–B
Least input increment Least command increment
Metric mm 0.001mm(Diameter) 0.0005mm system ma-
ma­chine
Inch mm 0.001mm(Diameter) 0.00005inch ma­chine
chine system
input
inch 0.0001inch(Diameter) 0.0005mm input
input
inch 0.0001inch(Diameter) 0.00005inch input
0.001mm(Radius) 0.001mm
0.001deg 0.001deg
0.0001inch(Radius) 0.001mm
0.001deg 0.001deg
0.001mm(Radius) 0.0001inch
0.001deg 0.001deg
0.0001inch(Radius) 0.0001inch
0.001deg 0.001deg
T able 2.3 (b) Increment system IS–C
Least input increment Least command increment
Metric mm 0.0001mm(Diameter) 0.00005mm system ma-
ma­chine
Inch mm 0.0001mm(Diameter) 0.000005inch ma­chine
chine system
input
inch 0.00001inch(Diameter) 0.00005mm input
input
inch 0.00001inch(Diameter) 0.000005inch input
0.0001mm(Radius) 0.0001mm
0.0001deg 0.0001deg
0.00001inch(Radius) 0.0001mm
0.0001deg 0.0001deg
0.0001mm(Radius) 0.00001inch
0.0001deg 0.0001deg
0.00001inch(Radius) 0.00001inch
0.0001deg 0.0001deg
Whether the least command increment is measured in millimeters or inches depends on the machine. Select either the increment in advance according to the setting of parameter INM (No.1001#0). A G code (G20 or G21) or a setting parameter can be used to toggle the least command increment between millimeter input and inch input.
30
B–63604EN/01
PROGRAMMING
2. CONTROLLED AXES
An axis in the metric system cannot be used together with a one in the inch system, or vice versa. In addition, some features such as circular interpolation and tool–nose radius compensation cannot be used for both axes in different units. For the unit to be set, refer to the manual supplied by the machine manufacturer.
2.4

MAXIMUM STROKES

The maximum stroke controlled by this CNC is shown in the table below: Maximum stroke=Least command increment"99999999
T able 2.4 Maximum strokes
Increment system
Metric machine
IS–B
IS–C
system Inch machine
system Metric machine
system Inch machine
system
Maximum strokes
"99999.999 mm "99999.999 deg
"9999.9999 inch "99999.999 deg
"9999.9999 mm "9999.9999 deg
"999.99999 inch "9999.9999 deg
NOTE
1 The unit in the table is a diameter value with diameter
programming and a radius value in radius programming.
2 A command exceeding the maximum stroke cannot be
specified.
3 The actual stroke depends on the machine tool.
31
3. PREPARATORY FUNCTION (G FUNCTION)

PREPARATORY FUNCTION (G FUNCTION)

3
PROGRAMMING
A number following address G determines the meaning of the command for the concerned block. G codes are divided into the following two types.
Type Meaning
One–shot G code The G code is effective only in the block in which it is
specified
Modal G code The G code is effective until another G code of the same
group is specified.
(Example) G01 and G00 are modal G codes.
B–63604EN/01
G01X_;
Z_; X_;
G00Z_;
There are three G code systems : A,B, and C (Table 3). Select a G code system using bits 6 (GSB) and 7 (GSC) of parameter 3401. T o use G code system B or C, the corresponding option is needed. Generally, this manual describes the use of G code system A, except when the described item can use only G code system B or C. ln such cases, the use of G code system B or C is described.
G01 is effective in this range
32
B–63604EN/01
PROGRAMMING
3. PREPARATORY FUNCTION (G FUNCTION)
Explanations
1. If the CNC enters the clear state (see bit 6 (CLR) of parameter 3402) when the power is turned on or the CNC is reset, the modal G codes change as follows.
(1)G codes marked with in Table 3 are enabled. (2)When the system is cleared due to power–on or reset, whichever
specified, either G20 or G21, remains effective.
(3)Bit 7 of parameter No. 3402 can be used to specify whether G22
or G23 is selected upon power–on. Resetting the CNC to the clear state does not affect the selection of G22 or G23.
(4) Setting bit 0 (G01) of parameter 3402 determines which code,
either G00 or G01, is effective.
(5) Setting bit 3 (G91) of parameter 3402 determines which code,
either G90 or G91, is effective.
2. G codes of group 00 except G10 and G11 are single–shot G codes.
3. P/S larm (No.010) is displayed when a G code not listed in the G code list is specified or a G code without a corresponding option is specified.
4. G codes of different groups can be specified in the same block. If G codes of the same group are specified in the same block, the G code specified last is valid.
5. If a G code of group 01 is specified in a canned cycle, the canned cycle is canceled in the same way as when a G80 command is specified. G codes of group 01 are not affected by G codes for specifying a canned cycle.
6. When G code system A is used, absolute or incremental programming is specified not by a G code (G90/G91) but by an address word (X/U, Z/W, C/H, Y/V). When G code system A is used for a drilling cycle, only the initial level is provided at the return point.
7. G codes are displayed for each group number.
33
3. PREPARATORY FUNCTION (G FUNCTION)
G code
A B C
G00 G00 G00 G01 G01 G01 Linear interpolation (Cutting feed) G02 G02 G02 G03 G03 G03 Circular interpolation CCW G04 G04 G04 Dwell G05 G05 G05 High speed remote buffer A
G07.1
(G107)
G10 G10 G10 Programmable data input
G11 G11 G11 Programmable data input cancel
G12.1
(G112)
G13.1
(G113)
G17 G17 G17 XpYp plane selection G18 G18 G18
G19 G19 G19 YpZp plane selection G20 G20 G70 Input in inch G21 G21 G71 G22 G22 G22 G23 G23 G23 G25 G25 G25 G26 G26 G26 G27 G27 G27 Reference position return check G28 G28 G28 Return to reference position G30 G30 G30 G31 G31 G31 Skip function G32 G33 G33 Thread cutting G34 G34 G34 G36 G36 G36 Automatic tool compensation X G37 G37 G37 G40 G40 G40 G41 G41 G41 G42 G42 G42 Tool nose radius compensation right
G50 G92 G92 Coordinate system setting or max. spindle speed setting G50.3 G92.1 G92.1 G50.2
(G250)
G51.2
(G251)
G07.1
(G107)
G12.1
(G112)
G13.1
(G113)
G50.2
(G250)
G51.2
(G251)
G07.1
(G107)
G12.1
(G112)
G13.1
(G113)
G50.2
(G250)
G51.2
(G251)
PROGRAMMING
T able 3 G code list (1/3)
Group Function
Positioning (Rapid traverse)
01
00
21
16
06
09
08
00
01
00
07
00
20
Circular interpolation CW
Cylindrical interpolation
Polar coordinate interpolation mode
Polar coordinate interpolation cancel mode
ZpXp plane selection
Input in mm Stored stroke check function on Stored stroke check function off Spindle speed fluctuation detection off Spindle speed fluctuation detection on
2nd, 3rd and 4th reference position return
Variable–lead thread cutting
Automatic tool compensation Z Tool nose radius compensation cancel Tool nose radius compensation left
Workpiece coordinate system preset Polygonal turning cancel
Polygonal turning
B–63604EN/01
34
B–63604EN/01
A B C G52 G52 G52 Local coordinate system setting G53 G53 G53 G54 G54 G54 G55 G55 G55 Workpiece coordinate system 2 selection G56 G56 G56 Workpiece coordinate system 3 selection G57 G57 G57 G58 G58 G58 Workpiece coordinate system 5 selection G59 G59 G59 Workpiece coordinate system 6 selection G65 G65 G65 00 Macro calling G66 G66 G66 Macro modal call
G67 G67 G67
G68 G68 G68 Mirror image for double turrets ON or balance cut mode
G69 G69 G69
G70 G70 G72 Finishing cycle G71 G71 G73 Stock removal in turning G72 G72 G74 G73 G73 G75 Pattern repeating G74 G74 G76 End face peck drilling G75 G75 G77 Outer diameter/internal diameter drilling G76 G76 G78 Multiple threading cycle G80 G80 G80 G83 G83 G83 Cycle for face drilling G84 G84 G84 Cycle for face tapping G86 G86 G86 G87 G87 G87 Cycle for side drilling G88 G88 G88 Cycle for side tapping G89 G89 G89 Cycle for side boring G90 G77 G20 Outer diameter/internal diameter cutting cycle G92 G78 G21 01 Thread cutting cycle G94 G79 G24 Endface turning cycle G96 G96 G96 Constant surface speed control G97 G97 G97 G98 G94 G94 Per minute feed G99
* G90 G90 * G91 G91 * G98 G98 Return to initial level (See Explanations 6) * G99 G99
G code
G95 G95
3. PREPARATORY FUNCTION
PROGRAMMING
T able 3 G code list (2/3)
Group Function
00
14
12
04
00
10
02
05
03
11
Machine coordinate system setting Workpiece coordinate system 1 selection
Workpiece coordinate system 4 selection
Macro modal call cancel
Mirror image for double turrets OFF or balance cut mode cancel
Stock removal in facing
Canned cycle for drilling cancel
Cycle for face boring
Constant surface speed control cancel
Per revolution feed Absolute programming Incremental programming
Return to R point level (See Explanations 6)
(G FUNCTION)
35
3. PREPARATORY FUNCTION (G FUNCTION)
G code
A B C G100 G100 G100 B axis control–Program registration completion G101 G101 G101 B axis control–First program registration start G102 G102 G102 00 B axis control–Second program registration start G103 G103 G103 B axis control–Third program registration start G110 G110 G110 B axis control–One motion operation programming
PROGRAMMING
T able 3 G code list (3/3)
Group Function
B–63604EN/01
36
B–63604EN/01
4
PROGRAMMING

INTERPOLATION FUNCTIONS

4. INTERPOLATION FUNCTIONS
37
PROGRAMMING4. INTERPOLATION FUNCTIONS
B–63604EN/01
4.1

POSITIONING (G00)

Format
Explanations
The G00 command moves a tool to the position in the workpiece system specified with an absolute or an incremental command at a rapid traverse rate. In the absolute command, coordinate value of the end point is programmed. In the incremental command the distance the tool moves is programmed.
G00IP_;
IP_: For an absolute command, the coordinates of an end
position, and for an incremental command, the distance the tool moves.
Either of the following tool paths can be selected according to bit 1 (LRP) of parameter No. 1401.
D Nonlinear interpolation positioning
The tool is positioned with the rapid traverse rate for each axis separately. The tool path is normally straight.
D Linear interpolation positioning
The tool path is the same as in linear interpolation (G01). The tool is positioned within the shortest possible time at a speed that is not more than the rapid traverse rate for each axis. However, the tool path is not the same as in linear interpolation (G01).
Linear interpolation positioning
End position
Non linear interpolation positioning
Start position
The rapid traverse rate in the G00 command is set to the parameter No.1420 for each axis independently by the machine tool builder. In the positioning mode actuated by G00, the tool is accelerated to a predetermined speed at the start of a block and is decelerated at the end of a block. Execution proceeds to the next block after confirming the in–position. “In–position” means that the feed motor is within the specified range. This range is determined by the machine tool builder by setting to parameter No.1826.
38
B–63604EN/01
Examples
PROGRAMMING
X
56.0
4. INTERPOLATION FUNCTIONS
30.5
30.0
Restrictions
φ40.0
Z
< Radius programming >
G00X40.0Z56.0 ; (Absolute command)
or
G00U–60.0W–30.5;(Incremental command)
The rapid traverse rate cannot be specified in the address F. Even if linear interpolation positioning is specified, nonlinear interpolation positioning is used in the following cases. Therefore, be careful to ensure that the tool does not foul the workpiece.
D G28 specifying positioning between the reference and intermediate
positions.
D G53
39
PROGRAMMING4. INTERPOLATION FUNCTIONS
B–63604EN/01
4.2

LINEAR INTERPOLATION (G01)

Format
Explanations
Tools can move along a line.
G01 IP_F_;
IP_: For an absolute command, the coordinates of an end
point , and for an incremental command, the distance the tool moves.
F_: Speed of tool feed (Feedrate)
A tools move along a line to the specified position at the feedrate specified in F. The feedrate specified in F is effective until a new value is specified. It need not be specified for each block. The feedrate commanded by the F code is measured along the tool path. If the F code is not commanded, the feedrate is regarded as zero. For feed–per–minute mode under 2–axis simultaneous control, the feedrate for a movement along each axis as follows :
Examples
D Linear interpolation
G01ααββ
< Diameter programming >
G01X40.0Z20.1F20 ; (Absolute command) or G01U20.0W–25.9F20 ; (Incremental command)
Ff ;
Feed rate of α axis direction :
Feed rate of β axis direction :
2
Ǹ
L + a2) b
X
20.1
Fa +
F
+
b
46.0
a
L
b
L
f
f
40
φ40.0
End point
Start point
φ20.0
Z
B–63604EN/01
PROGRAMMING
4. INTERPOLATION FUNCTIONS
4.3

CIRCULAR INTERPOLATION (G02, G03)

Format
The command below will move a tool along a circular arc.
Arc in the XpYp plane
G17
G02 G03
Arc in the ZpXp plane
G18
G02 G03
Arc in the YpZp plane
G02
G19
G03
Xp_Yp_
Xp_Zp_
Yp_Zp_
I_J_ R_
I_K_ R_
J_K_
R_
F_
F_
F_
Table.4.3 Description of the command format
Command Description
G17 Specification of arc on XpYp plane G18 Specification of arc on ZpXp plane G19 Specification of arc on Y pZp plane G02 Circular Interpolation Clockwise direction (CW) G03 Circular Interpolation Counterclockwise direction (CCW)
X
p_
Y
p_
Z
p_
I_ Xp axis distance from the start point to the center of an arc with
J_ Yp axis distance from the start point to the center of an arc with
Command values of X axis or its parallel axis (set by parameter No. 1022)
Command values of Y axis or its parallel axis (set by parameter No. 1022)
Command values of Z axis or its parallel axis (set by parameter No. 1022)
sign, radius value
sign, radius value
k_ Zp axis distance from the start point to the center of an arc with
sign, radius value R_ Arc radius with no sign (always with radius value) F_ Feedrate along the arc
41
Explanations
PROGRAMMING4. INTERPOLATION FUNCTIONS
B–63604EN/01
NOTE
The U–, V–, and W–axes (parallel with the basic axis) can be used with G–codes B and C.
D Direction of the circular
interpolation
D Distance moved on an
arc
D Distance from the start
point to the center of arc
Clockwise(G02) and counterclockwise(G03) on the X
plane or YpZp plane) are defined when the XpYp plane is viewed
(Z
pXp
in the positive–to–negative direction of the Z
axis (Yp axis or Xp axis,
p
pYp
plane
respectively) in the Cartesian coordinate system. See the figure below.
Yp
G02
G17
G03
Xp
Xp
G03
G02
Zp
G18
Zp
G02
G19
G03
Yp
The end point of an arc is specified by address Xp, Yp or Zp, and is expressed as an absolute or incremental value according to G90 or G91. For the incremental value, the distance of the end point which is viewed from the start point of the arc is specified.
The arc center is specified by addresses I, J, and K for the Xp, Y p, and Zp axes, respectively . The numerical value following I, J, or K, however, is a vector component in which the arc center is seen from the start point, and is always specified as an incremental value irrespective of G90 and G91, as shown below. I, J, and K must be signed according to the direction.
D Full–circle programming
End point (x,y)
yx
x
Center
Start
i
point
j
End point (z,x)
z
Center
End point (y ,z)
z
k
Start point
i
y
Center
Start
j
point
k
I0,J0, and K0 can be omitted. If the difference between the radius at the start point and that at the end point exceeds the value in a parameter (No.3410), an P/S alarm (No.020) occurs.
When X
p, Yp
, and Z
are omitted (the end point is the same as the start
p
point) and the center is specified with I, J, and K, a 360° arc (circle) is specified.
42
B–63604EN/01
PROGRAMMING
4. INTERPOLATION 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 considered. An arc with a sector angle of 180
°, and the other is more than 180° are
°or wider cannot be
specified. If Xp, Yp, and Zp are all omitted, if the end point is located at the same position as the start point and when R is used, an arc of 0
°is
programmed G02R ; (The cutter does not move.)
For arc (1) (less than 180°)
G02 W60.0 U10.0 R50.0
For arc (2) (greater than 180°)
An arc with a sector angle of 180°
or wider cannot be specified within a single block.
F300.0 ;
(2)
Start point
r=50mm
End point
(1)
r=50mm
X
D Feedrate
Restrictions
D Simultaneously
specifying R with I, J, and K
D Specifying an axis that is
not contained in the specified plane
D Difference in the radius
between the start and end points
Z
The feedrate in circular interpolation is equal to the feed rate specified by the F code, and the feedrate along the arc (the tangential feedrate of the arc) is controlled to be the specified feedrate. The error between the specified feedrate and the actual tool feedrate is
±2% or less. However, this feed rate is measured along the arc after the
tool nose radius compensation is applied
If I, J, K, and R addresses are specified simultaneously, the arc specified by address R takes precedence and the other are ignored.
If an axis not contained in the specified plane is commanded, an alarm is displayed. For example, when a ZX plane is specified in G–code B or C, specifying the X–axis or U–axis (parallel to the X–axis) causes P/S alarm No. 028 to be generated.
If the difference in the radius between the start and end points of the arc exceeds the value specified in parameter No. 3410, P/S alarm No. 020 is generated. If the end point is not on the arc, the tool moves in a straight line along one of the axes after reaching the end point.
43
PROGRAMMING4. INTERPOLATION FUNCTIONS
B–63604EN/01
D Specifying a semicircle
with R
If an arc having a central angle approaching 180 is specified with R, the calculation of the center coordinates may produce an error . In such a case, specify the center of the arc with I, J, and K.
Examples
D Command of circular
interpolation X, Z
G02X_Z_I_K_F_; G03X_Z_I_K_F_;
End point
X–axis
X
Z
Center of arc
K
(Absolute programming)
(Diameter programming)
Start point
Z–axis Z–axis Z–axis
End point
X–axis X–axis
X
Z
(Absolute programming)
G02X_Z_R_F_;
End point
(Diameter programming)
Start point
K
R
X
Z
Center of arc
(Diameter programming)
Start point
(Absolute programming)
X
15.0
R25.0
(Diameter programming)
G02X50.0Z30.0I25.0F0.3; or G02U20.0W–020.0I25.0F0.3; or G02X50.0Z30.0R25.0F0.3 or
10.0
G02U20.0W–20.0R25.F0.3;
φ50.0
30.0
Z
50.0
44
B–63604EN/01
PROGRAMMING
4. INTERPOLATION FUNCTIONS
4.4

POLAR COORDINA TE INTERPOLATION (G12.1, G13.1)

Format
D Specify G12.1 and G13.1
in Separate Blocks.
Explanations
D Polar coordinate
interpolation plane
Polar coordinate interpolation is a function that exercises contour control in converting a command programmed in a Cartesian coordinate system to the movement of a linear axis (movement of a tool) and the movement of a rotary axis (rotation of a workpiece). This method is useful in cutting a front surface and grinding a cam shaft on a lathe.
G12.1 ;
G13.1 ;
Starts polar coordinate interpolation mode (enables polar coordinate interpolation)
Specify linear or circular interpolation using coordinates in a Cartesian coordinate system consisting of a linear axis and rotary axis (virtual axis).
Polar coordinate interpolation mode is cancelled (for not performing polar coordinate interpolation)
G1 12 and G113 can be used in place of G12.1 and G13.1, respectively.
G12.1 starts the polar coordinate interpolation mode and selects a polar coordinate interpolation plane (Fig. 4.4 (a)). Polar coordinate interpolation is performed on this plane.
Rotary axis (virtual axis) (unit:mm or inch)
Linear axis (unit:mm or inch)
Origin of the workpiece coordinate system
Fig4.4 (a) Polar coordinate interpolation plane.
When the power is turned on or the system is reset, polar coordinate interpolation is canceled (G13.1). The linear and rotation axes for polar coordinate interpolation must be set in parameters (No. 5460 and 5461) beforehand.
CAUTION
The plane used before G12.1 is specified (plane selected by G17, G18, or G19) is canceled. It is restored when G13.1 (canceling polar coordinate interpolation) is specified. When the system is reset, polar coordinate interpolation is canceled and the plane specified by G17, G18, or G19 is used.
45
PROGRAMMING4. INTERPOLATION FUNCTIONS
B–63604EN/01
D Distance moved and
feedrate for polar coordinate interpolation
The unit for coordinates on the hypothetical axis is the same as the unit for the linear axis (mm/inch)
The unit for the feedrate is mm/min or inch/min
D G codes which can be
specified in the polar coordinate interpolation mode
D Circular interpolation in
the polar coordinate plane
In the polar coordinate interpolation mode, program commands are specified with Cartesian coordinates on the polar coordinate interpolation plane. The axis address for the rotation axis is used as the axis address for the second axis (virtual axis) in the plane. Whether a diameter or radius is specified for the first axis in the plane is the same as for the rotation axis regardless of the specification for the first axis in the plane. The virtual axis is at coordinate 0 immediately after G12.1 is specified. Polar interpolation is started assuming the angle of 0 for the position of the tool when G12.1 is specified. Specify the feedrate as a speed (relative speed between the workpiece and tool) tangential to the polar coordinate interpolation plane (Cartesian coordinate system) using F.
G01 Linear interpolation. . . . . . . . . . . .
G02, G03 Circular interpolation. . . . . . . . .
G04 Dwell. . . . . . . . . . . . . .
G40, G41, G42 Tool nose radius compensation . . . .
(Polar coordinate interpolation is applied to the path after cutter compensation.)
G65, G66, G67 Custom macro command. . . .
G98, G99 Feed per minute, feed per revolution. . . . . . . . .
The addresses for specifying the radius of an arc for circular interpolation (G02 or G03) in the polar coordinate interpolation plane depend on the first axis in the plane (linear axis).
D I and J in the Xp–Y p plane when the linear axis is the X–axis or an axis
parallel to the X–axis.
D J and K in the Yp–Zp plane when the linear axis is Yaxis or an axis
parallel to the Y–axis.
D K and I in the Zp–Xp plane when the linear axis is the Z–axis or an axis
parallel to the Z–axis.
D Movement along axes
not in the polar coordinate interpolation plane in the polar coordinate interpolation mode
D Current position display
in the polar coordinate interpolation mode
The radius of an arc can be specified also with an R command.
NOTE
The U–, V–, and W–axes (parallel with the basic axis) can be used with G–codes B and C.
The tool moves along such axes normally, independent of polar coordinate interpolation.
Actual coordinates are displayed. However, the remaining distance to move in a block is displayed based on the coordinates in the polar coordinate interpolation plane (Cartesian coordinates).
46
B–63604EN/01
Restrictions
PROGRAMMING
4. INTERPOLATION FUNCTIONS
Coordinate system for the
D
polar coordinate interpolation
D Tool nose radius
compensation command
D Program restart D Cutting feedrate for the
rotation axis
Before G12.1 is specified, a workpiece coordinate system) where the center of the rotary axis is the origin of the coordinate system must be set. In the G12.1 mode, the coordinate system must not be changed (G92, G52, G53, relative coordinate reset, G54 through G59, etc.).
The polar coordinate interpolation mode cannot be started or terminated (G12.1 or G13.1) in the tool nose radius compensation mode (G41 or G42). G12.1 or G13.1 must be specified in the tool nose radius compensation canceled mode (G40).
For a block in the G12.1 mode, the program cannot be restarted. Polar coordinate interpolation converts the tool movement for a figure
programmed in a Cartesian coordinate system to the tool movement in the rotation axis (C–axis) and the linear axis (X–axis). When the tool moves closer to the center of the workpiece, the C–axis component of the feedrate becomes larger and may exceed the maximum cutting feedrate for the C–axis (set in parameter (No. 1422)), causing an alarm (see the figure below). To prevent the C–axis component from exceeding the maximum cutting feedrate for the C–axis, reduce the feedrate specified with address F or create a program so that the tool (center of the tool when tool nose radius compensation is applied) does not move close to the center of the workpiece.
WARNING
Consider lines L1, L2, and L3. X is the distance the tool moves
θ1
θ2
θ3
X
L1
per time unit at the feedrate specified with address F in the Cartesian coordinate system. As the tool moves from L1 to L2 to L3, the angle at which the tool moves per time unit corresponding to X in the Cartesian coordinate system increases fromθ1 toθ 2
L2
to θ3.
L3
In other words, the C–axis component of the feedrate becomes larger as the tool moves closer to the center of the workpiece. The C component of the feedrate may exceed the maximum cutting feedrate for the C–axis because the tool movement in the Cartesian coordinate system has been converted to the tool movement for the C–axis and the X–axis.
L :Distance (in mm) between the tool center and workpiece center when the tool center is the
nearest to the workpiece center R :Maximum cutting feedrate (deg/min) of the C axis Then, a speed specifiable with address F in polar coordinate interpolation can be given by the formula below. Specify a speed allowed by the formula. The formula provides a theoretical value; in practice, a value slightly smaller than a theoretical value may need to be used due to a calculation error.
π
F < L × R ×
180
(mm/min)
D Diameter and radius
programming
Even when diameter programming is used for the linear axis (X–axis), radius programming is applied to the rotary axis (C–axis).
47
PROGRAMMING4. INTERPOLATION FUNCTIONS
B–63604EN/01
Examples
Example of Polar Coordinate Interpolation Program Based on X Axis (Linear Axis) and C Axis (Rotary Axis)
C (hypothetical axis)
N204
N205
N206
C axis
N203
N202
N208
N207
Path after tool nose radius compensation
Program path
N201
N200
X axis
Tool
Z axis
X axis is by diameter programming, C axis is by radius programming.
O0001 ;
N010 T0101
N0100 G00 X120.0 C0 Z _ ; Positioning to start position N0200 G12.1 ; Start of polar coordinate interpolation N0201 G42 G01 X40.0 F _ ; N0202 C10.0 ; N0203 G03 X20.0 C20.0 R10.0 ; N0204 G01 X–40.0 ; Geometry program N0205 C–10.0 ; (program based on cartesian coordinates on N0206 G03 X–20.0 C–20.0 I10.0 J0 ; X–C’ plane) N0207 G01 X40.0 ; N0208 C0 ; N0209 G40 X120.0 ; N0210 G13.1 ; Cancellation of polar coordinate interpolation N0300 Z __ ; N0400 X __C __ ;
N0900M30 ;
48
B–63604EN/01
PROGRAMMING
4. INTERPOLATION FUNCTIONS
4.5

CYLINDRICAL INTERPOLATION (G07.1)

Format
Explanations
D Plane selection
(G17, G18, G19)
The amount of travel of a rotary axis specified by an angle is once internally converted to a distance of a linear axis along the outer surface so that linear interpolation or circular interpolation can be performed with another axis. After interpolation, such a distance is converted back to the amount of travel of the rotary axis. The cylindrical interpolation function allows the side of a cylinder to be developed for programming. So programs such as a program for cylindrical cam grooving can be created very easily.
G07.1 IP r ; Starts the cylindrical interpolation mode
(enables cylindrical interpolation).
: : :
G07.1 IP 0 ; The cylindrical interpolation mode is cancelled.
IP : An address for the rotation axis
r : The radius of the cylinder
Specify G07.1 IP r ; and G07.1 IP 0; in separate blocks. G107 can be used instead of G07.1.
Use parameter No. 1002 to specify whether the rotation axis is the X–, Y–, or Z–axis, or an axis parallel to one of these axes. Specify the G code to select a plane for which the rotation axis is the specified linear axis. For example, when the rotation axis is an axis parallel to the X–axis, G17 must specify an Xp–Y p plane, which is a plane defined by the rotation axis and the Y–axis or an axis parallel to the Y–axis. Only one rotation axis can be set for cylindrical interpolation.
D Feedrate
NOTE
The U–, V–, and W–axes (parallel with the basic axis) can be used with G–codes B and C.
A feedrate specified in the cylindrical interpolation mode is a speed on the developed cylindrical surface.
49
PROGRAMMING4. INTERPOLATION FUNCTIONS
B–63604EN/01
D Circular interpolation
(G02,G03)
D Cutter compensation
D Cylindrical interpolation
accuracy
In the cylindrical interpolation mode, circular interpolation is possible with the rotation axis and another linear axis. Radius R is used in commands in the same way as described in Section 4.4. The unit for a radius is not degrees but millimeters (for metric input) or inches (for inch input). < Example Circular interpolation between the Z axis and C axis >
For the C axis of parameter No. 1022, 5 (axis parallel with the X axis) is to be set. In this case, the command for circular interpolation is
G18 Z__C__;
G02 (G03) Z__C__R__; For the C axis of parameter No. 1022, 6 (axis parallel with the Y axis) may be specified instead. In this case, however, the command for circular interpolation is
G19 C__Z__;
G02 (G03) Z__C__R__;
To perform cutter compensation in the cylindrical interpolation mode, cancel any ongoing cutter compensation mode before entering the cylindrical interpolation mode. Then, start and terminate cutter compensation within the cylindrical interpolation mode.
In the cylindrical interpolation mode, the amount of travel of a rotary axis specified by an angle is once internally converted to a distance of a linear axis on the outer surface so that linear interpolation or circular interpolation can be performed with another axis. After interpolation, such a distance is converted back to an angle. For this conversion, the amount of travel is rounded to a least input increment. So when the radius of a cylinder is small, the actual amount of travel can differ from a specified amount of travel. Note, however , that such an error is not accumulative. If manual operation is performed in the cylindrical interpolation mode with manual absolute on, an error can occur for the reason described above.
Restrictions
D Arc radius specification
in the cylindrical interpolation mode
D Circular interpolation
and tool nose radius compensation
The actual amount of travel
MOTION REV
R
MOTION REV
=
2×2πR
The amount of travel per rotation of the rotation axis (Set-
:
ting value of parameter No. 1260)
:
Workpiece radius
: Rounded to the least input increment
Specified value
2×2πR
MOTION REV
In the cylindrical interpolation mode, an arc radius cannot be specified with word address I, J, or K.
If the cylindrical interpolation mode is started when tool nose radius compensation is already applied, circular interpolation is not correctly performed in the cylindrical interpolation mode.
50
B–63604EN/01
PROGRAMMING
4. INTERPOLATION FUNCTIONS
D Positioning
D Coordinate system
setting
D Cylindrical interpolation
mode setting
D Canned cycle for drilling
during cylindrical interpolation mode
D Mirror Image for Double
Turret
In the cylindrical interpolation mode, positioning operations (including those that produce rapid traverse cycles such as G28, G80 through G89) cannot be specified. Before positioning can be specified, the cylindrical interpolation mode must be cancelled. Cylindrical interpolation (G07.1) cannot be performed in the positioning mode (G00).
In the cylindrical interpolation mode, a workpiece coordinate system G50 cannot be specified.
In the cylindrical interpolation mode, the cylindrical interpolation mode cannot be reset. The cylindrical interpolation mode must be cancelled before the cylindrical interpolation mode can be reset.
Canned cycles for drilling, G81 to G89, cannot be specified during cylindrical interpolation mode.
Mirror image for double turret, G68 and G69, cannot be specified during cylindrical interpolation mode.
51
Examples
PROGRAMMING4. INTERPOLATION FUNCTIONS
B–63604EN/01
mm
120
110
90 70
60
Example of a Cylindrical Interpolation Program
O0001 (CYLINDRICAL INTERPOLATION ); N01 G00 Z100.0 C0 ; N02 G01 G18 W0 H0 ; N03 G07.1 H57299 ; N04 G01 G42 Z120.0 D01 F250 ; N05 C30.0 ; N06 G02 Z90.0 C60.0 R30.0 ; N07 G01 Z70.0 ; N08 G03 Z60.0 C70.0 R10.0 ; N09 G01 C150.0 ; N10 G03 Z70.0 C190.0 R75.0 ; N1 1 G01 Z110.0 C230.0 ; N12 G02 Z120.0 C270.0 R75.0 ; N13 G01 C360.0 ; N14 G40 Z100.0 ; N15 G07.1 C0 ; N16 M30 ;
Z
N0 5
N06
N07
N08
N09
N12
N11
N10
N13
C
RZ
deg
C
0
30
60 70
150
230190
270
360
52
B–63604EN/01
PROGRAMMING
4. INTERPOLATION FUNCTIONS
4.6

CONSTANT LEAD THREADING (G32)

Fig. 4.6 (a) Straight thread
Format
T apered screws and scroll threads in addition to equal lead straight threads can be cut by using a G32 command. The spindle speed is read from the position coder on the spindle in real time and converted to a cutting feedrate for feed–per minute mode, which is used to move the tool.
L
L
Fig. 4.6 (b) T apered screw
L
Fig. 4.6 (c) Scroll thread
G32IP_F_;
IP_: End point F_: Lead of the long axis
(always radius programming)
Explanations
X axis
End point
δ
X
0
Fig. 4.6 (d) Example of thread cutting
2
Z
α
δ
1
L
Start point
Z axis
In general, thread cutting is repeated along the same tool path in rough cutting through finish cutting for a screw. Since thread cutting starts when the position coder mounted on the spindle outputs a 1–turn signal, threading is started at a fixed point and the tool path on the workpiece is unchanged for repeated thread cutting. Note that the spindle speed must remain constant from rough cutting through finish cutting. If not, incorrect thread lead will occur.
53
PROGRAMMING4. INTERPOLATION FUNCTIONS
X
Tapered thread
LX
α
LZ
αx45° lead is LZ αy45° lead is LX
Fig. 4.6 (e) LZ and LX of a tapered thread
B–63604EN/01
Z
In general, the lag of the servo system, etc. will produce somewhat incorrect leads at the starting and ending points of a thread cut. To compensate for this, a threading length somewhat longer than required should be specified. Table 4.6 lists the ranges for specifying the thread lead.
T able. 4.6 Ranges of lead sizes that can be specified
Least command increment
mm input 0.0001 to 500.0000mm
Inch input 0.000001 inch to 9.999999inch
54
B–63604EN/01
Explanations
1. Straight thread cutting
X axis
PROGRAMMING
30mm
4. INTERPOLATION FUNCTIONS
The following values are used in programming : Thread lead :4mm
δ1=3mm δ
=1.5mm
2
Depth of cut :1mm (cut twice) (Metric input, Diameter programming)
δ
2
2. Tapered thread cutting
X axis
φ50
δ
2
φ43
0
30
70
40
δ
1
G00 U–62.0 ; G32 W–74.5 F4.0 ;
Z axis
G00 U62.0 ;
W74.5 ; U–64.0 ;
(For the second cut, cut 1mm more) G32 W–74.5 ; G00 U64.0 ;
W74.5 ;
The following values are used in programming : Thread lead : 3.5mm in the direction of the Z axis
δ1=2mm δ
=1mm
2
Cutting depth in the X axis direction is 1mm (Cut twice) (Metric input, Diameter programming)
G00 X 12.0 Z72.0 ;
δ
1
Z axis
φ14
G32 X 41.0 Z29.0 F3.5 ; G00 X 50.0 ;
Z 72.0 ; X 10.0 ;
(Cut 1mm more for the second cut) G32 X 39.0 Z29.0 ; G00 X 50.0 ;
Z 72.0 ;
55
PROGRAMMING4. INTERPOLATION FUNCTIONS
B–63604EN/01
WARNING
1 Feedrate override is effective (fixed at 100%) during thread cutting. 2 it is very dangerous to stop feeding the thread cutter without stopping the spindle. This will
suddenly increase the cutting depth. Thus, the feed hold function is ineffective while thread cutting. If the feed hold button is pressed during thread cutting, the tool will stop after a block not specifying thread cutting is executed as if the SINGLE BLOCK button were pushed. However, the feed hold lamp (SPL lamp) lights when the FEED HOLD button on the machine control panel is pushed. Then, when the tool stops, the lamp is turned off (Single Block stop status).
3 When the FEED HOLD button is held down, or is pressed again in the first block that does not
specify thread cutting immediately after a thread cutting block, the tool stops at the block that does not specify thread cutting.
4 When thread cutting is executed in the single block status, the tool stops after execution of the
first block not specifying thread cutting.
5 When the mode was changed from automatic operation to manual operation during thread
cutting, the tool stops at the first block not specifying thread cutting as when the feed hold button is pushed as mentioned in Note 3. However, when the mode is changed from one automatic operation mode to another, the tool stops after execution of the block not specifying thread cutting as for the single block mode in Note 4.
6 When the previous block was a thread cutting block, cutting will start immediately without
waiting for detection of the 1–turn signal even if the present block is a thread cutting block.
G32Z _ F_ ; Z _; (A 1–turn signal is not detected before this block.) G32 ; (Regarded as threading block.) Z_ F_ ;(One turn signal is also not detected.)
7 Because the constant surface speed control is effective during scroll thread or tapered screw
cutting and the spindle speed changes, the correct thread lead may not be cut. Therefore, do not use the constant surface speed control during thread cutting. Instead, use G97.
8 A movement block preceding the thread cutting block must not specify chamfering or corner
R. 9 A thread cutting block must not specifying chamfering or corner R. 10The spindle speed override function is disabled during thread cutting. The spindle speed is
fixed at 100%. 11Thread cycle retract function is ineffective to G32.
56
B–63604EN/01
PROGRAMMING
4. INTERPOLATION FUNCTIONS
4.7
VARIABLE–LEAD THREAD CUTTING (G34)
Format
Explanations
Specifying an increment or a decrement value for a lead per screw revolution enables variable–lead thread cutting to be performed.
Fig. 4.7 Variable–lead screw
G34 IP_F_K_;
IP : End point F : Lead in long K : Increment and decrement of lead per spindle revolution
itudinal axis direction at the start point
Address other than K are the same as in straight/taper thread cutting with G32. Table 4.7 lists a range of values that can be specified as K.
Examples
Table 4.7 Range of valid K values
Metric input "0.0001 to"500.0000 mm/rev
Inch input "0.000001 to"9.999999 inch/rev
P/S alarm (No. 14) is produced, for example, when K such that the value in Table 4.7 is exceeded is directed, the maximum value of lead is exceeded as a result of increase or decrease by K or the lead has a negative value.
WARNING
The Thread Cutting Cycle Retract is not effective for G34.
Lead at the start point: 8.0 mm Lead increment: 0.3 mm/rev
G34 Z–72.0 F8.0 K0.3 ;
57
PROGRAMMING4. INTERPOLATION FUNCTIONS
B–63604EN/01
4.8

CONTINUOUS THREAD CUTTING

Explanations
This function for continuous thread cutting is such that fractional pulses output to a joint between move blocks are overlapped with the next move for pulse processing and output (block overlap) . Therefore, discontinuous machining sections caused by the interruption of move during continuously block machining are eliminated, thus making it possible to continuously direct the block for thread cutting instructions.
Since the system is controlled in such a manner that the synchronism with the spindle does not deviate in the joint between blocks wherever possible, it is possible to performed special thread cutting operation in which the lead and shape change midway.
G32
G32
Fig. 4.8 Continuous thread cutting
G32
Even when the same section is repeated for thread cutting while changing the depth of cut, this system allows a correct machining without impairing the threads.
NOTE
1 Block overlap is effective even for G01 command,
producing a more excellent finishing surface.
2 When extreme micro blocks continue, no block overlap may
function.
58
B–63604EN/01
PROGRAMMING
4. INTERPOLATION FUNCTIONS
4.9
MULTIPLE–THREAD CUTTING
Format
Explanations
Using the Q address to specify an angle between the one–spindle–rotation signal and the start of threading shifts the threading start angle, making it possible to produce multiple–thread screws with ease.
Multiple–thread screws.
(constant–lead threading)
G32 IP_ F_ Q_ ; G32 IP_ Q_ ;
IP_ : End point
F_ : Lead in longitudinal direction Q_ : Threading start angle
D Available thread cutting
commands
Limitations
D Start angle
Start angle increment
D
D Specifiable start angle
range
D Multiple–thread cutting
(G76)
G32: Constant–lead thread cutting G34: Variable–lead thread cutting G76: Multiple–thread cutting cycle G92: Thread cutting cycle
The start angle is not a continuous–state (modal) value. It must be specified each time it is used. If a value is not specified, 0 is assumed.
The start angle (Q) increment is 0.001 degrees. Note that no decimal point can be specified. Example: For a shift angle of 180 degrees, specify Q180000. Q180.000 cannot be specified, because it contains a decimal point.
A start angle (Q) of between 0 and 360000 (in 0.001–degree units) can be specified. If a value greater than 360000 (360 degrees) is specified, it is rounded down to 360000 (360 degrees).
For the G76 multiple–thread cutting command, always use the FS15 tape format.
59
Examples
PROGRAMMING4. INTERPOLATION FUNCTIONS
Program for producing double–threaded screws (with start angles of 0 and 180 degrees)
G00 X40.0 ; G32 W–38.0 F4.0 Q0 ; G00 X72.0 ;
W38.0 ;
X40.0 ; G32 W–38.0 F4.0 Q180000 ; G00 X72.0 ;
W38.0 ;
B–63604EN/01
60
B–63604EN/01
PROGRAMMING
4. INTERPOLATION FUNCTIONS
4.10

SKIP FUNCTION (G31)

Format
Explanations
Linear interpolation can be commanded by specifying axial move following the G31 command, like G01. If an external skip signal is input during the execution of this command, execution of the command is interrupted and the next block is executed. The skip function is used when the end of machining is not programmed but specified with a signal from the machine, for example, in grinding. It is used also for measuring the dimensions of a workpiece. For details of how to use this function, refer to the manual supplied by the machine tool builder.
G31 IP_ ;
G31: One–shot G code (If is effective only in the block in which
it is specified)
The coordinate values when the skip signal is turned on can be used in a custom macro because they are stored in the custom macro system variable #5061 to #5068, as follows:
#5061 X axis coordinate value #5062 Z axis coordinate value #5063 3rd axis coordinate value #5064 4th axis coordinate value
WARNING
To increase the precision of the tool position when the skip signal is input, feedrate override, dry run, and automatic acceleration/deceleration is disabled for the skip function when the feedrate is specified as a feed per minute value. To enable these functions, set bit 7 (SKF) of parameter No. 6200 to 1. If the feedrate is specified as a feed per rotation value, feedrate override, dry run, and automatic acceleration/deceleration are enabled for the skip function, regardless of the setting of the SKF bit.
NOTE
1 If G31 command is issued while tool nose radius compensation is
applied, an P/S alarm of No.035 is displayed. Cancel the cutter compensation with the G40 command before the G31 command is specified.
2 For the high–speed skip option, executing G31 during feed–per–
rotation mode causes P/S alarm (No.211) to be generated.
61
Examples
D The next block to G31 is an
incremental command
PROGRAMMING4. INTERPOLATION FUNCTIONS
G31 W100.0 F100;
U50.0;
B–63604EN/01
U50.0
D The next block to G31 is an
absolute command for 1 axis
Skip signal is input here
X
Z
Fig.4.10(a) The next block is an incremental command
G31 Z200.00 F100;
X100.0;
Skip signal is input here
100.0
50.0
W100
Actual motion Motion without skip signal
X100.0
X200.0
D The next block to G31 is an
absolute command for 2 axes
Actual motion Motion without skip signal
Fig.4.10(b) The next block is an absolute command for 1 axis
G31 G90X200.0 F100;
X300.0 Z100.0;
X
Skip signal is input here
10 0
100 200 300
Fig 4.10(c) The next block is an absolute command for 2 axes
(300,100)
Actual motion Motion without skip signal
Z
62
B–63604EN/01
PROGRAMMING
4. INTERPOLATION FUNCTIONS
4.11

MULTISTAGE SKIP

Format
In a block specifying P1 to P4 after G31, the multistage skip function stores coordinates in a custom macro variable when a skip signal (4–point or 8–point ; 8–point when a high–speed skip signal is used) is turned on. Parameters No. 6202 to No. 6205 can be used to select a 4–point or 8–point (when a high–speed skip signal is used) skip signal. One skip signal can be set to match multiple Pn or Qn (n=1,2,3,4) as well as to match a Pn or Qn on a one–to–one basis. A skip signal from equipment such as a fixed–dimension size measuring instrument can be used to skip programs being executed. In plunge grinding, for example, a series of operations from rough machining to spark–out can be performed automatically by applying a skip signal each time rough machining, semi–fine machining, fine–machining, or spark–out operation is completed.
Move command
G31 IP __ F __ P __ ;
IP_ : End point F_ : Feedrate P_ : P1–P4
Dwell
G04 X (U, P)__ (Q__) ;
Explanations
D Correspondence to skip
signals
X(U, P)_ : Dwell time Q_ : Q1 – Q4
Multistage skip is caused by specifying P1, P2, P3, or P4 in a G31 block. For an explanation of selecting (P1, P2, P3, or P4), refer to the manual supplied by the machine tool builder. Specifying Q1, Q2, Q3, or Q4 in G04 (dwell command) enables dwell skip in a similar way to specifying G31. A skip may occur even if Q is not specified. For an explanation of selecting (Q1, Q2, Q3, or Q4), refer to the manual supplied by the machine tool builder.
Parameter Nos. 6202 to 6205 can be used to specify whether the 4–point or 8–point skip signal is used (when a high–speed skip signal is used). Specification is not limited to one–to–one correspondence. It is possible to specify that one skip signal correspond to two or more Pns or Qn’s (n=1, 2, 3, 4). Also, bits 0 (DS1) to 7 (DS8) of parameter No. 6206 can be used to specify dwell.
CAUTION
Dwell is not skipped when Qn is not specified and parameters DS1–DS8 (No. 6206#0–#7) are not set.
63
PROGRAMMING4. INTERPOLATION FUNCTIONS
B–63604EN/01
4.12

TORQUE LIMIT SKIP (G31 P99)

Format
Explanations
D G31 P99
With the motor torque limited (for example, by a torque limit command, issued through the PMC window), a move command following G31 P99 (or G31 P98) can cause the same type of cutting feed as with G01 (linear interpolation). With the issue of a signal indicating a torque limit has been reached (because of pressure being applied or for some other reason), a skip occurs. For details of how to use this function, refer to the manuals supplied by the machine tool builder.
G31 P99 IP_ F_ ; G31 P98 IP_ F_ ;
G31: One–shot G code (G code effective only in the block in which it is issued)
If the motor torque limit is reached, or a SKIP signal is received during execution of G31 P99, the current move command is aborted, and the next block is executed.
D G31 P98
D Torque limit command
D Custom macro system
variable
Limitations
D Axis command
If the motor torque limit is reached during execution of G31 P98, the current move command is aborted, and the next block is executed. The SKIP signal <X0004#7/Tool post 2 X0013#7> does not affect G31 P98. Entering a SKIP signal during the execution of G31 P98 does not cause a skip.
If a torque limit is not specified before the execution of G31 P99/98, the move command continues; no skip occurs even if a torque limit is reached.
When G31 P99/98 is specified, the custom macro variables hold the coordinates at the end of a skip. (See Section 4.9.) If a SKIP signal causes a skip with G31 P99, the custom macro system variables hold the coordinates based on the machine coordinate system when it stops, rather than those when the SKIP signal is entered.
Only one axis can be controlled in each block with G31 P98/99. If two or more axes are specified to be controlled in such blocks, or no axis command is issued, P/S alarm No. 015 is generated.
D Degree of servo error
D High–speed skip
When a signal indicating that a torque limit has been reached is input during execution of G31 P99/98, and the degree of servo error exceeds 32767, P/S alarm No. 244 is generated.
With G31 P99, a SKIP signal can cause a skip, but not a high–speed skip.
64
B–63604EN/01
PROGRAMMING
4. INTERPOLATION FUNCTIONS
D Simplified
synchronization and slanted axis control
D Speed control
D Consecutive commands
G31 P99/98 cannot be used for axes subject to simplified synchronization or the X–axis or Z–axis when under slanted axis control.
Bit 7 (SKF) of parameter No. 6200 must be set to disable dry run, override, and auto acceleration or deceleration for G31 skip commands.
Do not use G31 P99/98 in consecutive blocks.
WARNING
Always specify a torque limit before a G31 P99/98 command. Otherwise, G31 P99/98 allows move commands to be executed without causing a skip.
NOTE
If G31 is issued with tool nose radius compensation specified, P/S alarm No. 035 is generated. Therefore, before issuing G31, execute G40 to cancel tool nose radius compensation.
Examples
O0001 ;
: : Mjj ; : : G31 P99 X200. F100 ; : G01 X100. F500 ; : : MDD ; : : M30 ; : %
The PMC specifies the torque limit through the window.
Torque limit skip command Move command for which a torque
limit is applied
Torque limit canceled by the PMC
65
5

FEED FUNCTIONS

PROGRAMMING5. FEED FUNCTIONS
B–63604EN/01
66
B–63604EN/01
PROGRAMMING
5. FEED FUNCTIONS
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 operators 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
F
:Rapid traverse
F
R
0
R
rate
: Acceleration/
T
R
deceleration time constant for rapid traverse rate
Time
T
R
Feed rate
C
0
T
C
Fig. 5.1 (a) Automatic acceleration/deceleration (example)
T
R
F
: Feedrate
CF
: Acceleration/
T
C
T
C
deceleration time constant for a cut­ting feedrate
Time
67
PROGRAMMING5. FEED FUNCTIONS
B–63604EN/01
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)).
X
Programmed path Actual tool path
0
Fig. 5.1 (b) Example of tool path between two blocks
Z
In circular interpolation, a radial error occurs (Fig. 5.1(c)).
X
r:Error
Programmed path Actual tool path
r
0
Fig. 5.1 (c) Example of radial error in circular interpolation
Z
5.2

RAPID TRAVERSE

Format
Explanations
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.
G00 IP_ ;
G00 : G code (group 01) for positioning (rapid traverse) IP_ ; Dimension word for the end point
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 operators 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.
68
B–63604EN/01
PROGRAMMING
5. FEED FUNCTIONS
5.3

CUTTING FEED

Format
Explanations
Feedrate of linear interpolation (G01), circular interpolation (G02, G03), etc. are commanded with numbers after the F code. In cutting feed, the next block is executed so that the feedrate change from the previous block is minimized. Two modes of specification are available:
1. Feed per minute (G98) After F, specify the amount of feed of the tool per minute.
2. Feed per revolution (G99) After F, specify the amount of feed of the tool per spindle revolution.
Feed per minute
G98 ; G code (group 05) for feed per minute F_ ; Feedrate command (mm/min or inch/min)
Feed per revolution
G99 ; G code (group 05) for feed per revolution F_ ; Feedrate command (mm/rev or inch/rev)
D Tangential speed
constant control
D Feed per minute (G98)
Cutting feed is controlled so that the tangential feedrate is always set at a specified feedrate.
X
End point
F
Start point
Linear interpolation
Fig. 5.3 (a) T angential feedrate (F)
X
Starting point
F
Center End point
ZZ
Circular interpolation
After specifying G98 (in the feed per minute mode), the amount of feed of the tool per minute is to be directly specified by setting a number after F . G98 is a modal code. Once a G98 is specified, it is valid until G99 (feed per revolution) is specified. At power–on, the feed per revolution mode is set. An override from 0% to 254% (in 1% steps) can be applied to feed per minute with the switch on the machine operators panel. For detailed information, see the appropriate manual of the machine tool builder.
69
PROGRAMMING5. FEED FUNCTIONS
B–63604EN/01
D Feed per revolution
(G99)
F
Fig. 5.3 (b) Feed per minute
Feed amount per minute (mm/min or inch/min)
WARNING
No override can be used for some commands such as for threading.
After specifying G99 (in the feed per revolution mode), the amount of feed of the tool per spindle revolution is to be directly specified by setting a number after F . G99 is a modal code. Once a G99 is specified, it is valid until G98 (feed per minute) is specified. An override from 0% to 254% (in 1% steps) can be applied to feed per revolution with the switch on the machine operators panel. For detailed information, see the appropriate manual of the machine tool builder.
If bit 0 (NPC) of parameter No. 1402 has been set to 1, feed–per–rotation commands can be specified even when a position coder is not being used. (The CNC converts feed–per–rotation commands to feed–per–minute commands.)
D Cutting feedrate clamp
F
Fig. 5.3 (c) Feed per revolution
Feed amount per spindle revolution (mm/rev or inch/rev)
CAUTION
1 When the speed of the spindle is low, feedrate fluctuation
may occur. The slower the spindle rotates, the more frequently feedrate fluctuation occurs.
2 No override can be used for some commands such as for
threading.
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.
70
B–63604EN/01
PROGRAMMING
5. FEED FUNCTIONS
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:
D Reference
5.4

DWELL (G04)

Format
Explanations
See Appendix C for a range of feedrates that can be specified.
Dwell G04 X_ ; or G04 U_ ; or G04 P_ ;
X_ : Specify a time (decimal point permitted) U_ : Specify a time (decimal point permitted) P_ : Specify a time (decimal point not permitted)
By specifying a dwell, the execution of the next block is delayed by the specified time. Bit 1 (DWL) of parameter No. 3405 can specify dwell for each rotation in feed per rotation mode (G99).
Table 5.4 (a)
Command value range of the dwell time (Command by X or U)
Increment system Command value range Dwell time unit
IS–B 0.001 to 99999.999
s or rev
IS–C 0.0001 to 9999.9999
Table 5.4 (b)
Command value range of the dwell time (Command by P)
Increment system Command value range Dwell time unit
IS–B 1 to 99999999 0.001 s or rev IS–C 1 to 99999999 0.0001 s or rev
71
6
PROGRAMMING6. REFERENCE POSITION

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.
B–63604EN/01
72
B–63604EN/01
6.1

REFERENCE POSITION RETURN

PROGRAMMING
6. REFERENCE POSITION
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).
Y
2nd reference position
3rd reference position
Reference position
4th reference position
X
Machine zero point
Fig. 6.1 (a) Machine zero point and reference positions
73
PROGRAMMING6. REFERENCE POSITION
B–63604EN/01
D Reference position
return
D Reference position
return check
Tools are automatically moved to the reference 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.
X
Intermediate position
Reference position
Z
Fig. 6.2 (b) Reference position return
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.
Format
D Reference position
return
D Reference position
return check
G28 _ ;
IP
G30 P2 _ ; G30 P3 _ ; G30 P4 _ ;
IP_ : Command specifying the intermediate position
(Absolute/incremental command)
IPG27 _ ;
IP_ : Command specifying the reference position
(Absolute/incremental command)
Reference position return 2nd reference position return
IP
3rd reference position return
IP
4th reference position return
IP
(P2 can be omitted.)
74
B–63604EN/01
Explanations
PROGRAMMING
6. REFERENCE POSITION
D Reference position
return (G28)
D 2nd, 3rd, and 4th
reference position return (G30)
D Reference position
return check (G27)
Restrictions
D Status the machine lock
being turned on
Positioning to the intermediate or reference positions are performed at the rapid traverse rate of each axis. Therefore, for safety, the tool nose radius compensation, and tool offset should be cancelled before executing this command.
In a system without an absolute–position detector, the first, third, and fourth reference position return functions can be used only after the 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.
G27 command positions the tool at rapid traverse rate. If the tool reaches the reference position, the reference position return lamp lights up. However , if the position reached by the tool is not the reference position, 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.
D First return to the
reference position after the power has been turned on (without an absolute position detector)
D Reference position
return check in an offset mode
D Lighting the lamp when
the programmed position does not coincide with the reference position
Reference
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.
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 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 least input increment. This is because the least input increment of the machine is smaller than its least command increment.
D Manual reference
position return
See III–3.1.
75
7
PROGRAMMING7. COORDINATE SYSTEM

COORDINATE SYSTEM

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 two program axes, the X–axis and Z–axis, are used, coordinates are specified as follows:
X_Z_
This command is referred to as a dimension word.
B–63604EN/01
X
β
α
Z
Zero point
Fig. 7 T ool position specified by XαZβ
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_.
76
Loading...