fanuc 0i-MA Operators Manual

OPERATOR’S MANUAL

B-63514EN/01

Ȧ No part of this manual may be reproduced in any form. Ȧ All specifications and designs are subject to change without notice.

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

SAFETY PRECAUTIONS

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

Contents

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

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

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

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

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

s–1

SAFETY PRECAUTIONS

B–63514EN/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–63514EN/01

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–63514EN/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–63514EN/01

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 operator’s 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. Absolute/incremental mode

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

8. 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.

B–63514EN/01

9. Programmable mirror image

Note that programmed operations vary considerably when a programmable mirror image is enabled.

10.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–63514EN/01

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 operator’s 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 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.

4. 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.

5. 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

6. 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.

7. Software operator ’s panel and menu switches

Using the software operator’s panel and menu switches, in combination with the MDI panel, it is possible to specify operations not supported by the machine operator’s panel, such as mode change, override value change, and jog feed commands. Note, however, that if the MDI panel keys are operated inadvertently, the machine may behave unexpectedly, possibly damaging the tool, the machine itself, the workpiece, or causing injury to the user.

B–63514EN/01

8. 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.

9. 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.

10.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.

11. Cutter 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 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.

12.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–63514EN/01

1. Memory backup battery replacement

SAFETY PRECAUTIONS

W ARNINGS RELATED TO DAILY MAINTENANCE

WARNING

Only those personnel who have received approved safety and maintenance training may perform this work. When replacing the batteries, be careful not to touch the high–voltage circuits (marked fitted with an insulating cover). Touching the uncovered high–voltage circuits presents an extremely dangerous electric shock hazard.

and

NOTE

The CNC uses batteries to preserve the contents of its memory, because it must retain data such as programs, offsets, and parameters even while external power is not applied. If the battery voltage drops, a low battery voltage alarm is displayed on the machine operator’s panel or screen. When a low battery voltage alarm is displayed, replace the batteries within a week. Otherwise, the contents of the CNC’s memory will be lost. Refer to the maintenance section of the this manual for details of the battery replacement procedure.

s–9

SAFETY PRECAUTIONS

B–63514EN/01

WARNING

2. Absolute pulse coder battery replacement

NOTE

The absolute pulse coder uses batteries to preserve its absolute position. If the battery voltage drops, a low battery voltage alarm is displayed on the machine operator’s panel or screen. When a low battery voltage alarm is displayed, replace the batteries within a week. Otherwise, the absolute position data held by the pulse coder will be lost. Refer to the maintenance section of the this manual for details of the battery replacement procedure.

and

s–10

B–63514EN/01

3. Fuse replacement

SAFETY PRECAUTIONS

WARNING

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–63514EN/01

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

I. GENERAL

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

1.1 GENERAL FLOW OF OPERATION OF CNC MACHINE TOOL 6. . . . . . . . . . . . . . . . . . . . . . . . .

1.2 NOTES ON READING THIS MANUAL 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

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

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

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

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

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

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

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

Tool – Absolute, Incremental Commands 19. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

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

2.2 AXIS NAME 30. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

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

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

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

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

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

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

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

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

4.6 CYLINDRICAL INTERPOLATION (G07.1) 50. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.7 THREAD CUTTING (G33) 53. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8 SKIP FUNCTION (G31) 55. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.9 HIGH SPEED SKIP SIGNAL (G31) 57. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–1

Table of Contents

B–63514EN/01

5. FEED FUNCTIONS 58. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.1 GENERAL 59. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.2 RAPID TRAVERSE 61. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.3 CUTTING FEED 62. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4 CUTTING FEEDRATE CONTROL 65. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.1 Exact Stop (G09, G61) Cutting Mode (G64) Tapping Mode (G63) 66. . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.2 Automatic Corner Override 67. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.2.1 Automatic Override for Inner Corners (G62) 67. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.2.2 Internal Circular Cutting Feedrate Change 70. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.3 Automatic Corner Deceleration 71. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.3.1 Corner Deceleration According to the Corner Angle 71. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.3.2 Corner Deceleration According to the Feedrate Difference between

Blocks Along Each Axis 73. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.5 DWELL (G04) 75. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6. REFERENCE POSITION 76. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.1 REFERENCE POSITION RETURN 77. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7. COORDINATE SYSTEM 82. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1 MACHINE COORDINATE SYSTEM 83. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2 WORKPIECE COORDINATE SYSTEM 84. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.1 Setting a Workpiece Coordinate System 84. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.2 Selecting a W orkpiece Coordinate System 85. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.3 Changing Workpiece Coordinate System 86. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.4 W orkpiece Coordinate System Preset (G92.1) 89. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.5 Adding Workpiece Coordinate Systems (G54.1 or G54) 91. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.3 LOCAL COORDINATE SYSTEM 93. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.4 PLANE SELECTION 95. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8. COORDINATE VALUE AND DIMENSION 96. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1 ABSOLUTE AND INCREMENTAL PROGRAMMING (G90, G91) 97. . . . . . . . . . . . . . . . . . . . . . .

8.2 POLAR COORDINATE COMMAND (G15, G16) 98. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3 INCH/METRIC CONVERSION (G20,G21) 101. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4 DECIMAL POINT PROGRAMMING 102. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9. SPINDLE SPEED FUNCTION (S FUNCTION) 103. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1 SPECIFYING THE SPINDLE SPEED WITH A CODE 104. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2 SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY (S5–DIGIT COMMAND) 104. . . . . . . . .

9.3 CONSTANT SURFACE SPEED CONTROL (G96, G97) 105. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.TOOL FUNCTION (T FUNCTION) 108. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.1 TOOL SELECTION FUNCTION 109. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2 TOOL LIFE MANAGEMENT FUNCTION 110. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2.1 T ool Life Management Data 111. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2.2 Register, Change and Delete of Tool Life Management Data 112. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2.3 T ool Life Management Command in a Machining Program 115. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2.4 T ool Life 118. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–2

B–63514EN/01

Table of Contents

11.AUXILIARY FUNCTION 119. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1 AUXILIARY FUNCTION (M FUNCTION) 120. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2 MULTIPLE M COMMANDS IN A SINGLE BLOCK 121. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3 THE SECOND AUXILIARY FUNCTIONS (B CODES) 122. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.PROGRAM CONFIGURATION 123. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.1 PROGRAM COMPONENTS OTHER THAN PROGRAM SECTIONS 125. . . . . . . . . . . . . . . . . . . . .

12.2 PROGRAM SECTION CONFIGURATION 128. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.3 SUBPROGRAM (M98, M99) 134. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.FUNCTIONS TO SIMPLIFY PROGRAMMING 138. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1 CANNED CYCLE 139. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.1 High–Speed Peck Drilling Cycle (G73) 143. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.2 Left–Handed T apping Cycle (G74) 145. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.3 Fine Boring Cycle (G76) 147. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.4 Drilling Cycle, Spot Drilling (G81) 149. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.5 Drilling Cycle Counter Boring Cycle (G82) 151. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.6 Peck Drilling Cycle (G83) 153. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.7 Small–Hole Peck Drilling Cycle (G83) 155. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.8 T apping Cycle (G84) 159. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.9 Boring Cycle (G85) 161. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.10 Boring Cycle (G86) 163. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.11 Boring Cycle Back Boring Cycle (G87) 165. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.12 Boring Cycle (G88) 167. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.13 Boring Cycle (G89) 169. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.14 Canned Cycle Cancel (G80) 171. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.2 RIGID TAPPING 174. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.2.1 Rigid Tapping (G84) 175. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.2.2 Left–Handed Rigid T apping Cycle (G74) 178. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.2.3 Peck Rigid T apping Cycle (G84 or G74) 181. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.2.4 Canned Cycle Cancel (G80) 183. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.3 OPTIONAL ANGLE CHAMFERING AND CORNER ROUNDING 184. . . . . . . . . . . . . . . . . . . . . . .

13.4 EXTERNAL MOTION FUNCTION (G81) 187. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.5 INDEX TABLE INDEXING FUNCTION 188. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.COMPENSATION FUNCTION 191. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1 TOOL LENGTH OFFSET (G43, G44, G49) 192. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.1 General 192. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.2 G53, G28, and G30 Commands in T ool Length Offset Mode 197. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2 AUTOMATIC TOOL LENGTH MEASUREMENT (G37) 200. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3 TOOL OFFSET (G45–G48) 204. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4 OVERVIEW OF CUTTER COMPENSATION C (G40–G42) 209. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5 DETAILS OF CUTTER COMPENSATION C 215. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.1 General 215. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.2 T ool Movement in Start–up 216. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.3 T ool Movement in Of fset Mode 220. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.4 T ool Movement in Of fset Mode Cancel 234. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.5 Interference Check 240. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.6 Overcutting by Cutter Compensation 245. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.7 Input Command from MDI 248. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–3

Table of Contents

14.5.8 G53, G28, G30 and G29 Commands in Cutter Compensation C Mode 249. . . . . . . . . . . . . . . . . . . . . . . .

14.5.9 Corner Circular Interpolation (G39) 268. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–63514EN/01

14.6 TOOL COMPENSATION VALUES, NUMBER OF COMPENSATION VALUES,

AND ENTERING VALUES FROM THE PROGRAM (G10) 270. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.7 SCALING (G50, G51) 272. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.8 COORDINATE SYSTEM ROTATION (G68, G69) 277. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.9 NORMAL DIRECTION CONTROL (G40.1, G41.1, G42.1 OR G150, G151, G152) 283. . . . . . . . . . .

14.10 PROGRAMMABLE MIRROR IMAGE (G50.1, G51.1) 288. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.CUSTOM MACRO 290. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1 VARIABLES 291. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2 SYSTEM VARIABLES 295. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3 ARITHMETIC AND LOGIC OPERATION 303. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.4 MACRO STATEMENTS AND NC STATEMENTS 308. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.5 BRANCH AND REPETITION 309. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.5.1 Unconditional Branch (GOTO Statement) 309. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.5.2 Conditional Branch (IF Statement) 309. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.5.3 Repetition (While Statement) 310. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6 MACRO CALL 313. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.1 Simple Call (G65) 314. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.2 Modal Call (G66) 318. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.3 Macro Call Using G Code 320. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.4 Macro Call Using an M Code 321. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.5 Subprogram Call Using an M Code 322. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.6 Subprogram Calls Using a T Code 323. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6.7 Sample Program 324. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.7 PROCESSING MACRO STATEMENTS 326. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.8 REGISTERING CUSTOM MACRO PROGRAMS 328. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.9 LIMITATIONS 329. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.10 EXTERNAL OUTPUT COMMANDS 330. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.11 INTERRUPTION TYPE CUSTOM MACRO 334. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.11.1 Specification Method 335. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.11.2 Details of Functions 336. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.PATTERN DATA INPUT FUNCTION 344. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.1 DISPLAYING THE PATTERN MENU 345. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.2 PATTERN DATA DISPLAY 349. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.3 CHARACTERS AND CODES TO BE USED

FOR THE PATTERN DATA INPUT FUNCTION 353. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

17.PROGRAMMABLE PARAMETER ENTRY (G10) 355. . . . . . . . . . . . . . . . . . . . . . . . . . .

18.MEMORY OPERATION USING FS10/11 TAPE FORMAT 357. . . . . . . . . . . . . . . . . . .

19.HIGH SPEED CUTTING FUNCTIONS 358. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19.1 FEEDRATE CLAMPING BY ARC RADIUS 359. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19.2 LOOK–AHEAD CONTROL (G08) 360. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19.3 LOOK–AHEAD CONTROL (MULTIPLE BLOCKS ARE READ IN ADVANCE) (G05.1) 362. . . . .

c–4

B–63514EN/01

Table of Contents

20.AXIS CONTROL FUNCTIONS 367. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.1 SIMPLE SYNCHRONOUS CONTROL 368. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20.2 ROTARY AXIS ROLL–OVER 371. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

III. OPERATION

1. GENERAL 375. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.1 MANUAL OPERATION 376. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.2 TOOL MOVEMENT BY PROGRAMING–AUTOMATIC OPERATION 378. . . . . . . . . . . . . . . . . . . .

1.3 AUTOMATIC OPERATION 379. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4 TESTING A PROGRAM 381. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4.1 Check by Running the Machine 381. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4.2 How to View the Position Display Change without Running the Machine 382. . . . . . . . . . . . . . . . . . . . . .

1.5 EDITING A PART PROGRAM 383. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.6 DISPLAYING AND SETTING DATA 384. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7 DISPLAY 387. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.1 Program Display 387. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.2 Current Position Display 388. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.3 Alarm Display 388. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.4 Parts Count Display, Run Time Display 389. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.5 Graphic Display 389. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.8 DATA INPUT/OUTPUT 390. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2. OPERATIONAL DEVICES 391. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1 SETTING AND DISPLAY UNITS 392. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.1 9” Monochrome CRT/MDI Unit 393. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.2 8.4” Color LCD/MDI Unit 393. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.3 Key Location of MDI 394. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.2 EXPLANATION OF THE KEYBOARD 395. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3 FUNCTION KEYS AND SOFT KEYS 397. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.1 General Screen Operations 397. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.2 Function Keys 398. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.3 Soft Keys 399. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.4 Key Input and Input Buffer 415. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.5 W arning Messages 416. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.6 Soft Key Configuration 416. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4 EXTERNAL I/O DEVICES 417. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.1 F ANUC Handy File 419. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5 POWER ON/OFF 420. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.1 Turning on the Power 420. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.2 Screen Displayed at Power–on 421. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.3 Power Disconnection 422. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3. MANUAL OPERATION 423. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.1 MANUAL REFERENCE POSITION RETURN 424. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.2 JOG FEED 426. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.3 INCREMENTAL FEED 428. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.4 MANUAL HANDLE FEED 429. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.5 MANUAL ABSOLUTE ON AND OFF 432. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–5

Table of Contents

B–63514EN/01

4. AUT OMATIC OPERATION 437. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.1 MEMORY OPERATION 438. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.2 MDI OPERATION 440. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.3 DNC OPERATION 444. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.4 PROGRAM RESTART 446. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

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

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

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

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

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

5.1 MACHINE LOCK AND AUXILIARY FUNCTION LOCK 468. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

8.3 FILE DELETION 494. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4 PROGRAM INPUT/OUTPUT 495. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.1 Inputting a Program 495. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.2 Outputting a Program 498. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5 OFFSET DATA INPUT AND OUTPUT 500. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5.1 Inputting Offset Data 500. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5.2 Outputting Offset Data 501. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6 INPUTTING AND OUTPUTTING PARAMETERS AND

PITCH ERROR COMPENSATION DATA 502. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.1 Inputting Parameters 502. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.2 Outputting Parameters 503. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.3 Inputting Pitch Error Compensation Data 504. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.4 Outputting Pitch Error Compensation Data 505. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.7 INPUTTING/OUTPUTTING CUSTOM MACRO COMMON VARIABLES 506. . . . . . . . . . . . . . . . .

8.7.1 Inputting Custom Macro Common Variables 506. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.7.2 Outputting Custom Macro Common Variable 507. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–6

B–63514EN/01

Table of Contents

8.8 DISPLAYING DIRECTORY OF FLOPPY CASSETTE 508. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.1 Displaying the Directory 509. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.2 Reading Files 512. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.3 Outputting Programs 513. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.4 Deleting Files 514. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.9 OUTPUTTING A PROGRAM LIST FOR A SPECIFIED GROUP 516. . . . . . . . . . . . . . . . . . . . . . . . .

8.10 DATA INPUT/OUTPUT ON THE ALL IO SCREEN 517. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.10.1 Setting Input/Output–Related Parameters 518. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.10.2 Inputting and Outputting Programs 519. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.10.3 Inputting and Outputting Parameters 524. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.10.4 Inputting and Outputting Offset Data 526. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.10.5 Outputting Custom Macro Common Variables 528. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.10.6 Inputting and Outputting Floppy Files 529. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9. EDITING PROGRAMS 534. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1 INSERTING, ALTERING AND DELETING A WORD 535. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.1 W ord Search 536. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.2 Heading a Program 538. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.3 Inserting a W ord 539. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.4 Altering a W ord 540. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.5 Deleting a W ord 541. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2 DELETING BLOCKS 542. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.1 Deleting a Block 542. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.2 Deleting Multiple Blocks 543. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3 PROGRAM NUMBER SEARCH 544. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4 SEQUENCE NUMBER SEARCH 545. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5 DELETING PROGRAMS 547. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.1 Deleting One Program 547. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.2 Deleting All Programs 547. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.3 Deleting More than One Program by Specifying a Range 548. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6 EXTENDED PART PROGRAM EDITING FUNCTION 549. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.1 Copying an Entire Program 550. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.2 Copying Part of a Program 551. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.3 Moving Part of a Program 552. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.4 Merging a Program 553. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.5 Supplementary Explanation for Copying, Moving and Merging 554. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6.6 Replacement of W ords and Addresses 556. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.7 EDITING OF CUSTOM MACROS 558. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.8 BACKGROUND EDITING 559. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.9 PASSWORD FUNCTION 560. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.CREATING PROGRAMS 562. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.1 CREATING PROGRAMS USING THE MDI PANEL 563. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2 AUTOMATIC INSERTION OF SEQUENCE NUMBERS 564. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.3 CREATING PROGRAMS IN TEACH IN MODE (PLAYBACK) 566. . . . . . . . . . . . . . . . . . . . . . . . . .

10.4 CONVERSATIONAL PROGRAMMING WITH GRAPHIC FUNCTION 569. . . . . . . . . . . . . . . . . . . .

1 1.SETTING AND DISPLA YING DAT A 573. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1 SCREENS DISPLAYED BY FUNCTION KEY

11.1.1 Position Display in the Work Coordinate System 581. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

POS

c–7

580. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Table of Contents

B–63514EN/01

11.1.2 Position Display in the Relative Coordinate System 582. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.3 Overall Position Display 584. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.4 Presetting the W orkpiece Coordinate System 585. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.5 Actual Feedrate Display 586. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.6 Display of Run Time and Parts Count 588. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.7 Operating Monitor Display 589. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2 SCREENS DISPLAYED BY FUNCTION KEY

PROG

(IN MEMORY MODE OR MDI MODE) 591. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.1 Program Contents Display 592. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.2 Current Block Display Screen 593. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.3 Next Block Display Screen 594. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.4 Program Check Screen 595. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.5 Program Screen for MDI Operation 596. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3 SCREENS DISPLAYED BY FUNCTION KEY

11.3.1 Displaying Memory Used and a List of Programs 597. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3.2 Displaying a Program List for a Specified Group 600. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4 SCREENS DISPLAYED BY FUNCTION KEY

11.4.1 Setting and Displaying the Tool Offset Value 604. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.2 T ool Length Measurement 606. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.3 Displaying and Entering Setting Data 608. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.4 Sequence Number Comparison and Stop 610. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.5 Displaying and Setting Run Time, Parts Count, and Time 612. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.6 Displaying and Setting the W orkpiece Origin Offset Value 614. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.7 Direct Input of Measured W orkpiece Origin Offsets 615. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.8 Displaying and Setting Custom Macro Common V ariables 617. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.9 Displaying Pattern Data and Pattern Menu 618. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.10 Displaying and Setting the Software Operator’s Panel 620. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.11 Displaying and Setting T ool Life Management Data 622. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.12 Displaying and Setting Extended T ool Life Management 625. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

PROG

(IN THE EDIT MODE) 597. . . . . . . . . . . . . . .

OFFSET SETTING

603. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5 SCREENS DISPLAYED BY FUNCTION KEY

SYSTEM

11.5.1 Displaying and Setting Parameters 631. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5.2 Displaying and Setting Pitch Error Compensation Data 633. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

AND WARNING MESSAGES FOR DATA SETTING OR INPUT/OUTPUT OPERATION 635. . . . .

11.6.1 Displaying the Program Number and Sequence Number 635. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.6.2 Displaying the Status and W arning for Data Setting or Input/Output Operation 636. . . . . . . . . . . . . . . . . .

11.7 SCREENS DISPLAYED BY FUNCTION KEY

MESSAGE

11.7.1 External Operator Message History Display 638. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8 CLEARING THE SCREEN 640. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8.1 Erase Screen Display 640. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8.2 Automatic Erase Screen Display 641. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.GRAPHICS FUNCTION 642. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.1 GRAPHICS DISPLAY 643. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.HELP FUNCTION 649. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

638. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–8

B–63514EN/01

Table of Contents

IV. MAINTENANCE

1. METHOD OF REPLACING BATTERY 657. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.1 REPLACING BATTERY FOR CONTROL UNIT 658. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.2 BATTERY FOR SEPARATE ABSOLUTE PULSE CODERS (6 VDC) 660. . . . . . . . . . . . . . . . . . . . . .

1.3 BATTERY FOR BUILT–IN ABSOLUTE PULSE CODERS (6 VDC) 661. . . . . . . . . . . . . . . . . . . . . .

APPENDIX

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

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

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

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

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

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

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

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

E. STATUS WHEN TURNING POWER ON, WHEN CLEAR

AND WHEN RESET 692. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

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

c–9

I. GENERAL

B–63514EN/01

GENERAL

This manual consists of the following parts:

1. GENERAL

About this manual

I. GENERAL

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

II. PROGRAMMING

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

III. OPERATION

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

IV. MAINTENANCE

Describes procedures for replacing batteries.

APPENDIX

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

Some functions described in this manual may not be applied to some products. For detail, refer to the DESCRIPTIONS manual(B–63502EN).

This manual does not describe parameters in detail. For details on parameters mentioned in this manual, refer to the manual for parameters (B–63510EN).

Special symbols

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 0i–MA 0i–MA Series 0i

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.

1. GENERAL

GENERAL

B–63514EN/01

Related manuals

The table below lists manuals related to MODEL A of Series 0i. In the table, this manual is marked with an asterisk (*).

T able 1 Related Manuals

Manual name

DESCRIPTIONS B–63502EN CONNECTION MANUAL (HARDWARE) B–63503EN CONNECTION MANUAL (FUNCTION) B–63503EN–1 OPERATOR’S MANUAL (For LATHE) B–63504EN OPERATOR’S MANUAL (For MACHINING CENTER) B–63514EN * MAINTENANCE MANUAL B–63505EN P ARAMETER MANUAL B–63510EN PROGRAMMING MANUAL

(Macro Compiler / Macro Executer) FAPT MACRO COMPILER PROGRAMMING MANUAL B–66102E

Specification

number

B–61803E–1

Related manuals of SERVO MOTOR α series, β series

Manual name

FANUC AC SER VO MOTOR α series DESCRIPTIONS B–65142E FANUC AC SER VO MOTOR α series PARAMETER

MANUAL FANUC AC SPINDLE MOT OR α series DESCRIPTIONS B–65152E FANUC AC SPINDLE MOT OR α series PARAMETER

MANUAL FANUC SER VO AMPLIFIER α series DESCRIPTIONS B–65162E FANUC SER VO MOT OR α series MAINTENANCE

MANUAL FANUC SER VO MOT OR β series DESCRIPTIONS B–65232EN FANUC SER VO MOT OR β series MAINTENANCE

MANUAL FANUC SER VO MOT OR β series (I/O Link Option)

MAINTENANCE MANUAL

Specification

number

B–65150E

B–65160E

B–65165E

B–65235EN

B–65245EN

B–63514EN/01

Related manuals of OPEN CNC

GENERAL

1. GENERAL

Related manuals of OPEN CNC

Manual name

FANUC OPEN CNC OPERATOR’S MANUAL (Basic Operation Package 1 (for Windows 95/NT))

FANUC OPEN CNC OPERATOR’S MANUAL (DNC Operation Management Package)

Specification

number

B–62994EN

B–63214EN

1. GENERAL

GENERAL

B–63514EN/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 OPERATION

Part programming

CNC

MACHINE TOOL

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

1. Determination of workpieces machining range

2. Method of mounting workpieces on the machine tool

3. Machining sequence in every machining process

4. Machining tools and machining

Decide the machining method in every machining process.

Machining process

Machining procedure

1. Machining method : Rough Semi Finish

2. Machining tools

3. Machining conditions : Feedrate Cutting depth

4. Tool path

1 2 3

Feed cutting Side cutting

Hole

machining

B–63514EN/01

GENERAL

Tool

Side cutting

1. GENERAL

Face cutting

Hole machining

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

1. GENERAL

1.2 NOTES ON READING THIS MANUAL

GENERAL

NOTE

1 The function of an CNC machine tool system depends not

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

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

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

3 Machining programs, parameters, variables, etc. are stored

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

4 This manual describes as many reasonable variations in

equipment usage as possible. It cannot address every combination of features, options and commands that should not be attempted. If a particular combination of operations is not described, it should not be attempted.

B–63514EN/01

II. PROGRAMMING

B–63514EN/01

GENERAL

PROGRAMMING

1. GENERAL

PROGRAMMING

B–63514EN/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).

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

Tool

Workpiece

Program G01 X_ _ Y_ _ ; X_ _ ;

D Tool movement along an

arc

Fig. 1.1 (a) T ool movement along a straight line

Program G03X_ _Y_ _R_ _;

Tool

Workpiece

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

B–63514EN/01

PROGRAMMING

1. GENERAL

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

(a) Movement along straight line

G01 Y_ _; X– –Y– – – –;

Control unit

Interpolation

a)Movement

along straight line

b)Movement

along arc

Fig. 1.1 (c) Interpolation function

(b) Movement along arc

G03X––Y––R––;

X axis

Y axis

Tool movement

NOTE

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

1. GENERAL

PROGRAMMING

B–63514EN/01

1.2 FEED–FEED FUNCTION

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

mm/min

Workpiece

Table

Fig. 1.2 (a) Feed function

Tool

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

B–63514EN/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.

Reference position

Tool

Workpiece

Table

Fig. 1.3.1 (a) Reference position

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

Reference position return is performed by manual button operation.

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

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

1. GENERAL

1.3.2

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

PROGRAMMING

B–63514EN/01

Program

Explanations

D Coordinate system

Part drawing

Fig. 1.3.2 (a)

Coordinate system

CNC

Command

Tool

Workpiece

Machine tool

Coordinate system

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

(1)Coordinate system on part drawing

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

(2)Coordinate system specified by the CNC

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

230

300

Program zero point

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

Present tool position

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

B–63514EN/01

PROGRAMMING

1. GENERAL

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

Coordinate system on part drawing established on the work-

Coordinate system specified by the CNC established on the table

Table

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

systemon part drawing

Workpiece

piece

D Methods of setting the

two coordinate systems in the same position

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

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

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

Fixed distance

Program zero point

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

Workpiece’s standard point

Fixed distance

1. GENERAL

PROGRAMMING

B–63514EN/01

(2)Mounting a workpiece directly against the jig

Program zero point

Jig

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

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

pallet on the jig

Pallet

Jig

Workpiece

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

B–63514EN/01

1.3.3

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

PROGRAMMING

1. GENERAL

Explanations

D Absolute command

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

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

Command specifying movement from point A to point B

B(10.0,30.0,20.0)

G90 X10.0 Y30.0 Z20.0 ;

Coordinates of point B

Tool

D Incremental command

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

Tool

X=40.0

Z=–10.0

Command specifying movement from point A to point B

Y=–30.0

G91 X40.0 Y–30.0 Z–10.0

Distance and direction for movement along each axis

;

1. GENERAL

PROGRAMMING

B–63514EN/01

1.4 CUTTING SPEED – SPINDLE SPEED FUNCTION

Examples

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

Tool

Spindle speed N

rpm

Workpiece

T ool diameter

f D mm

V: Cutting speed

m/min

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

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

B–63514EN/01

PROGRAMMING

1. GENERAL

1.5 SELECTION OF T OOL USED FOR VARIOUS MACHINING – TOOL FUNCTION

Examples

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

Tool number

01 02

ATC magazine

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

1. GENERAL

PROGRAMMING

B–63514EN/01

1.6 COMMAND FOR MACHINE OPERATIONS – MISCELLANEOUS FUNCTION

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

Tool

Coolant

Workpiece

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

B–63514EN/01

PROGRAMMING

1. GENERAL

1.7 PROGRAM CONFIGURATION

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

Block

Tool movement sequence

Block

Program

Fig. 1.7 (a) Program configuration

Block

⋅ ⋅ ⋅ ⋅

Block

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

1. GENERAL

PROGRAMMING

B–63514EN/01

Explanations

D Block

D Program

The block and the program have the following configurations.

1 block

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

Sequence number

Preparatory function

Dimension word Miscel-

laneous function

Fig. 1.7 (b) Block configuration

Spindle function

Tool function

End of block

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

;

Offff;

⋅

M30 ;

Fig. 1.7 (c) Program configuration

Program number

Block Block Block

⋅

End of program

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

B–63514EN/01

PROGRAMMING

1. GENERAL

D Main program and

subprogram

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

Main program

⋅ ⋅

M98P1001

⋅

M98P1002

⋅

M98P1001

⋅

Subprogram #1

O1001

M99

Subprogram #2

O1002

Program for hole #1

Program for hole #2

⋅

M99

Hole #1

Hole #2

1. GENERAL

1.8 TOOL FIGURE AND TOOL MOTION BY PROGRAM

Explanations

PROGRAMMING

B–63514EN/01

D Machining using the end

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

D Machining using the side

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

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

Standard tool

Workpiece

H3 H4

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

Cutter path using cutter compensation

Machined part figure

Workpiece

Cutter

If radius of cutters are stored in the CNC (Data Display and Setting : see III–11), the tool can be moved by cutter radius apart from the machining part figure. This function is called cutter compensation (See III–14.4,

14.5).

B–63514EN/01

PROGRAMMING

1. GENERAL

1.9 TOOL MOVEMENT RANGE – STROKE

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

Table

Motor

Limit switch

Machine zero point

Specify these distances.

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

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

CONTROLLED AXES

PROGRAMMING2. CONTROLLED AXES

B–63514EN/01

2.1 CONTROLLED AXES

PROGRAMMING 2. CONTROLLED AXES

Item

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

Simultaneously controlled axes expansion (total) Max. 4 axes

Max. 4 axes (included in Cs axis)

0i–MA

NOTE

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

PROGRAMMING2. CONTROLLED AXES

B–63514EN/01

2.2 AXIS NAME

Limitations

D Default axis name

D Duplicate axis names

The names of three basic axes are always X, Y, and Z. The name of an additional axis can be set to A, B, C, U, V , or W by using parameter 1020. Parameter No. 1020 is used to determine the name of each axis. When this parameter is set to 0 or a character other than the valid characters is specified, an axis name from 1 to 4 is assigned by default.

When a default axis name (1 to 4) is used, operation in the MEM mode, MDI mode, and RMT mode is disabled.

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

B–63514EN/01

PROGRAMMING 2. CONTROLLED AXES

2.3 INCREMENT SYSTEM

The increment system consists of the least input increment (for input) and least command increment (for output). The least input increment is the least increment for programming the travel distance. The least command increment is the least increment for moving the tool on the machine. Both increments are represented in mm, inches, or deg. The increment system is classified into IS–B and IS–C. Select IS–B or IS–C using bit 1 (ISC) of parameter 1004. The setting of bit 1 (ISC) of parameter No.1004 applies to all axes. When IS–C is selected, for example, the increment system for all axes is set to IS–C.

Name of increment system

IS–B

IS–C

Least input increment

0.001mm

0.0001inch

0.001deg

0.0001mm

0.00001inch

0.0001deg

Least command increment

0.001mm

0.0001inch

0.001deg

0.0001mm

0.00001inch

0.0001deg

Maximum stroke

99999.999mm

9999.9999inch

99999.999deg

9999.9999mm

999.99999inch

9999.9999deg

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

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

PROGRAMMING2. CONTROLLED AXES

B–63514EN/01

2.4 MAXIMUM STROKE

Maximum stroke = Least command increment 99999999 See 2.3 Increment System.

T able 2.4 (a) Maximum strokes

Increment system

Metric machine system "99999.999 mm

IS–B

Inch machine system "9999.9999 inch

Metric machine system "9999.9999 mm

IS–C

Inch machine system "999.99999 inch

Maximum stroke

"99999.999 deg

"9999.9999 deg

NOTE

1 A command exceeding the maximum stroke cannot be

specified.

2 The actual stroke depends on the machine tool.

B–63514EN/01

3. PREPARATORY FUNCTION

PROGRAMMING

PREPARATORY FUNCTION (G FUNCTION)

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

Type Meaning

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

specified.

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

same group is specified.

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

(G FUNCTION)

G01X ;

Z; X;

G00Z

G01 is effective in this range.

;

3. PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING

B–63514EN/01

Explanations

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

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

indicated in Table 3.

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

power–up or reset.

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

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

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

No. 3402.

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

No. 3402.

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

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

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

3.When a G code not listed in the G code list is specified, P/S alarm No. 010 is output.

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

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

6.G codes are indicated by group.

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

B–63514EN/01

3. PREPARATORY FUNCTION

PROGRAMMING

T able 3 G code list (1/3)

G code

G00

G01 G02 G03 Circular interpolation/Helical interpolation CCW G04 Dwell, Exact stop G05.1 Look–ahead control (Multiple blocks are read in advance) G07.1 (G107) Cylindrical interpolation G08 00 Look–ahead control G09 Exact stop G10 Programmable data input G11 Programmable data input mode cancel

G15 G16

G17

G18

G19 G20 Input in inch G21

G22 G23 G27 Reference position return check G28 Return to reference position G29 00 Return from reference position G30 2nd, 3rd and 4th reference position return G31 Skip function G33 01 Thread cutting G37 Automatic tool length measurment G39

G40 G41 G42 Cutter compensation right G40.1 (G150) G41.1 (G151) 18 Normal direction control left side on G42.1 (G152) Normal direction control right side on G43 Tool length compensation + direction G44 G45 Tool offset increase G46 Tool offset decrease

G47 G48 Tool offset double decrease

G49

Group Function

Positioning

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

08 Tool length compensation cancel

Linear interpolation Circular interpolation/Helical interpolation CW

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

YpZp plane selection Zp: Z axis or its parallel axis

Input in mm Stored stroke check function on Stored stroke check function off

Corner offset circular interpolation Cutter compensation cancel Cutter compensation left

Normal direction control cancel mode

Tool length compensation – direction

Tool offset double increase

(G FUNCTION)

3. PREPARATORY FUNCTION

(G FUNCTION)

G code

G50 G51

G50.1 G51.1 G52 Local coordinate system setting G53

G54 G54.1 Additional workpiece coordinate system selection

G55 G56 G57 Workpiece coordinate system 4 selection G58 Workpiece coordinate system 5 selection G59 Workpiece coordinate system 6 selection G60 00/01 Single direction positioning G61 Exact stop mode G62 Automatic corner override G63

G64 G65 00 Macro call G66 Macro modal call

G67

G68 Coordinate rotation

G69 G73 Peck drilling cycle G74

G76

G80 Canned cycle cancel/external operation function cancel G81

G82 Drilling cycle or counter boring cycle G83 Peck drilling cycle G84 G85 Boring cycle G86 Boring cycle G87 Back boring cycle G88 Boring cycle G89 Boring cycle

G90

G91 G92 G92.1

PROGRAMMING

T able 3 G code list (2/3)

Group Function

Scaling cancel Scaling Programmable mirror image cancel Programmable mirror image

Machine coordinate system selection Workpiece coordinate system 1 selection

Workpiece coordinate system 2 selection Workpiece coordinate system 3 selection

Tapping mode Cutting mode

Macro modal call cancel

Coordinate rotation cancel

Counter tapping cycle Fine boring cycle

Drilling cycle, spot boring cycle or external operation function

Tapping cycle

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

speed Workpiece coordinate system preset

B–63514EN/01

PROGRAMMING

T able 3 G code list (3/3)

G code

G94 G95 G96 Constant surface speed control

G97 G98 G99

Group Function

Feed per minute Feed per rotation

Constant surface speed control cancel Return to initial point in canned cycle Return to R point in canned cycle

3. PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING4. INTERPOLATION FUNCTIONS

INTERPOLATION FUNCTIONS

B–63514EN/01

4.1 POSITIONING (G00)

Format

PROGRAMMING

4. INTERPOLATION FUNCTIONS

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

G00 _;IP

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

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

Explanations

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

D Nonlinear interpolation positioning

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

D Linear interpolation positioning

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

Start position

Linear interpolation positioning

End position

Non linear interpolation positioning

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

PROGRAMMING4. INTERPOLATION FUNCTIONS

B–63514EN/01

Limitations

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

positions.

D G53

B–63514EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.2 SINGLE DIRECTION POSITIONING (G60)

Format

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

Overrun

Start position

End position

G60 _;

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

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

Temporary stop

Explanations

Examples

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

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

When one–shot G60 commands are used.

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

Single direction positioning

When modal G60 command is used.

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

Single direction positioning mode start

Single direction positioning

Single direction positioning mode cancel

PROGRAMMING4. INTERPOLATION FUNCTIONS

B–63514EN/01

Restrictions

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

effected in Z axis.

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

overrun has been set by the parameter.

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

positioning is not performed.

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

the canned cycles of G76 and G87.

B–63514EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.3

LINEAR INTERPOLATION (G01)

Format

Explanations

Tools can move along a line

G01 _F_;

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

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

F_:Speed of tool feed (Feedrate)

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

G01ααββγγζζ

Feed rate of α axis direction :

Feed rate of β axis direction :

Feed rate of γ axis direction :

Feed rate of ζ axis direction :

L + a2) b2) g2) z

Ff ;

Fa +

Fb+

Fg +

Fz+

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

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

PROGRAMMING4. INTERPOLATION FUNCTIONS

B–63514EN/01

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

Examples

D Linear interpolation

202) 40

The feed rate for the C axis is

300

0.14907

0.14907 (min)8

268.3 degńmin

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

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

Y axis

100.0

(End position)

D Feedrate for the

rotation axis

(Start position)

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

(End point)

200.00

(Start point)

90°

Feedrate is 300 deg/min

X axis

B–63514EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.4

CIRCULAR INTERPOLATION (G02, G03)

Format

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

Arc in the XpYp plane

G17

Arc in the ZpXpplane

G18

Arc in the YpZp plane

G19

G02 G03

Xp_Yp_

Xp_ p_

Yp_ Zp_

I_ J_ R_

I_ K_ R_

J_ K_

F_ ;

T able. 4.4 Description of the Command Format

Command

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

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

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

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

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

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

with sign

Description

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

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

Explanations

PROGRAMMING4. INTERPOLATION FUNCTIONS

B–63514EN/01

D Direction of the circular

interpolation

D Distance moved on an

arc

D Distance from the start

point to the center of arc

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

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

pXp

in the positive–to–negative direction of the Z

axis (Yp axis or Xp axis,

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

Yp Xp Zp

G18

G03

G02

G19

G02

G03

G02

G17

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

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

End point (x,y)

Center

Start point

End point (z,x)

Center

Start point

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

End point (y ,z)

Center

are omitted (the end

Start point

point is the same as the start point) and the center is specified with I, J, and K, a 360° arc (circle) is specified. G02I_; Command for a circle If the difference between the radius at the start point and that at the end point exceeds the permitted value in a parameter (No.3410), an P/S alarm (No.020) occurs.

B–63514EN/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°, and the other is more than 180° are considered. When an arc exceeding 180° is commanded, the radius must be specified with a negative value. If Xp, Yp, and Zp are all omitted, if the end point is located at the same position as the start point and when R is used, an arc of 0° is programmed G02R ; (The cutter does not move.)

For arc (1)(less than 180°)

G91 G02 XP60.0 YP20.0 R50.0 F300.0 ;

For arc (2)(greater than 180°)

G91 G02 X

60.0 YP20.0 R–50.0 F300.0 ;

r=50mm

End point

D Feedrate

Restrictions

Start point

r=50mm

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

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

PROGRAMMING4. INTERPOLATION FUNCTIONS

B–63514EN/01

Examples

Y axis

100

50R

140

60R

200

60 40

90 120

The above tool path can be programmed as follows ;

(1) In absolute programming

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

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

(2) In incremental programming

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

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

X axis

B–63514EN/01

4.5

HELICAL INTERPOLATION (G02, G03)

Format

PROGRAMMING

4. INTERPOLATION FUNCTIONS

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

Synchronously with arc of XpY p plane

Explanations

G17

Synchronously with arc of ZpXp plane

G18

Synchronously with arc of Y pZp plane

G19

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

G02 G03

Up to two other axes can be specified.

Xp_Yp_

Xp_Zp_

Yp_Zp_

I_J_ R_

I_K_

J_K_ R_

α_(β_)F_;

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

Length of linear axis

F×

Length of circular arc

Restrictions

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

Tool path

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

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

which a helical interpolation is commanded.

PROGRAMMING4. INTERPOLATION FUNCTIONS

B–63514EN/01

4.6

CYLINDRICAL INTERPOLATION (G07.1)

Format

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

G07.1 r ; Starts the cylindrical interpolation mode

(enables cylindrical interpolation).

: :

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

: An address for the rotation axis

r : The radius of the cylinder

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

IP IP

Explanations

D Plane selection

(G17, G18, G19)

D Feedrate

D Circular interpolation

(G02,G03)

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

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

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

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

G18 Z__C__;

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

G19 C__Z__;

G02 (G03) Z__C__R__;

B–63514EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

D Tool offset

D Cylindrical interpolation

accuracy

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

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

The actual amount of travel

MOTION REV

2×2πR

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

ting value of parameter No. 1260)

Workpiece radius

Specified value

2×2πR

MOTION REV

Limitations

D Arc radius specification

in the cylindrical interpolation mode

D Circular interpolation

and cutter compensation

D Positioning

D Coordinate system

setting

D Cylindrical interpolation

mode setting

:Rounded to the least input increment

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

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

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

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

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

D Tool offset

D Index table indexing

function

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

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

Examples

PROGRAMMING4. INTERPOLATION FUNCTIONS

B–63514EN/01

Example of a Cylindrical Interpolation Program

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

120 110

90 70

N05

N06

N07

N08 N09 N10

30 60 70

150

N11

N12

230190

270

N13

360

deg

B–63514EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.7

THREAD CUTTING (G33)

Format

Explanations

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

G33 _ F_ ; F : Long axis direction lead

Workpiece

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

mm input

Inch input

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

Least command

increment

0.001 mm F1 to F50000 (0.01 to 500.00mm)

0.0001 mm F1 to F50000 (0.01 to 500.00mm)

0.0001 inch

0.00001 inch

Command value range of the lead

F1 to F99999 (0.0001 to 9.9999inch)

NOTE

1 The spindle speed is limited as follows :

PROGRAMMING4. INTERPOLATION FUNCTIONS

B–63514EN/01

1 x spindle speed x

Maximum feedrate

Thread lead

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

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

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

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

is terminated)

Examples

Thread cutting at a pitch of 1.5mm

G33 Z10. F1.5;

B–63514EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.8

SKIP FUNCTION (G31)

Format

Explanations

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

G31 _ ;

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

is specified)

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

#5061 X axis coordinate value #5062 Y axis coordinate value #5063 Z axis coordinate value #5064 4th axis coordinate value

WARNING

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

NOTE

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

Examples D The next block to G31 is

an incremental command

PROGRAMMING4. INTERPOLATION FUNCTIONS

G31 G91X100.0 F100;

Y50.0;

B–63514EN/01

D The next block to G31 is

an absolute command for 1 axis

Skip signal is input here

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

G31 G90X200.00 F100;

Y100.0;

Skip signal is input here

100.0

50.0

Actual motion Motion without skip signal

Y100.0

X200.0

D The next block to G31 is

an absolute command for 2 axes

Actual motion Motion without skip signal

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

G31 G90X200.0 F100;

X300.0 Y100.0; Y

Skip signal is input here

100

100 200 300

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

(300,100)

Actual motion Motion without skip signal

B–63514EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.9 HIGH SPEED SKIP SIGNAL (G31)

Format

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

For details, refer to the appropriate manual supplied from the machine tool builder.

G31 IP_ ;

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

specified)

FEED FUNCTIONS

PROGRAMMING5. FEED FUNCTIONS

B–63514EN/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 operator’s panel.

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

Rapid traverse rate

: Rapid traverse

rate

: Acceleration/

deceleration time constant for rapid traverse rate

Feed rate

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

: Feedrate

: Acceleration/

deceleration time constant for a cutting feedrate

Time

PROGRAMMING5. FEED FUNCTIONS

B–63514EN/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)).

Programmed path Actual tool path

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

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

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

∆r:Error

Programmed path Actual tool path

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

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

the tool to move as programmed.

B–63514EN/01

5.2

RAPID TRAVERSE

Format

PROGRAMMING

G00 IP_ ;

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

5. FEED FUNCTIONS

Explanations

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

PROGRAMMING5. FEED FUNCTIONS

B–63514EN/01

5.3

CUTTING FEED

Format

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

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

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

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

Feed per minute

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

Feed per revolution

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

F1–digit feed

FN ; N : Number from 1 to 9

Explanations

D Tangential speed

constant control

D Feed per minute (G94)

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

End point

Start point

Linear interpolation

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

Starting point

Center End point

Circular interpolation

After specifying G94 (in the feed per minute mode), the amount of feed of the tool per minute is to be directly specified by setting a number after F . G94 is a modal code. Once a G94 is specified, it is valid until G95 (feed per revolution) is specified. At power–on, the feed per minute mode is set. An override from 0% to 254% (in 1% steps) can be applied to feed per minute with the switch on the machine operator’s panel. For detailed information, see the appropriate manual of the machine tool builder.

B–63514EN/01

PROGRAMMING

Workpiece

Table

Fig. 5.3 (b) Feed per minute

5. FEED FUNCTIONS

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

Tool

WARNING

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

D Feed per revolution

(G95)

After specifying G95 (in the feed per revolution mode), the amount of feed of the tool per spindle revolution is to be directly specified by setting a number after F . G95 is a modal code. Once a G95 is specified, it is valid until G94 (feed per minute) is specified. An override from 0% to 254% (in 1% steps) can be applied to feed per revolution with the switch on the machine operator’s panel. For detailed information, see the appropriate manual of the machine tool builder.

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

Fig. 5.3 (c) Feed per revolution

CAUTION

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

PROGRAMMING5. FEED FUNCTIONS

B–63514EN/01

D One–digit F code feed

D Cutting feedrate clamp

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

Fmax

∆

F +

100X

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

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

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

A common upper limit can be set on the cutting feedrate along each axis with parameter No. 1422. If an actual cutting feedrate (with an override applied) exceeds a specified upper limit, it is clamped to the upper limit. Parameter No. 1430 can be used to specify the maximum cutting feedrate for each axis only for linear interpolation and circular interpolation. When the cutting feedrate along an axis exceeds the maximum feedrate for the axis as a result of interpolation, the cutting feedrate is clamped to the maximum feedrate.

Reference

NOTE

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

See Appendix C for range of feedrate command value.

B–63514EN/01

PROGRAMMING

5. FEED FUNCTIONS

5.4

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

CUTTING FEEDRATE CONTROL

T able 5.4 Cutting Feedrate Control

Function name G code V alidity of G code Description

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

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

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

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

Exact stop G09

Exact stop mode G61

Cutting mode G64

Tapping mode G63

Automatic override for

inner corners Auto– matic

G62

This function is valid for specified blocks only.

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

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

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

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

Internal circular cutting

feedrate change

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

the G code.

NOTE

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

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

2 Inner corner angle θ: 2°

(α is a set value)

The internal circular cutting feedrate is changed.

< θ x α x 178°

Workpiece

Tool

Format

PROGRAMMING5. FEED FUNCTIONS

B–63514EN/01

5.4.1

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

Explanations

Exact stop G09 IP_ ; Exact stop mode G61 ;

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

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

(2)

(1)

Position check Tool path in the exact stop mode

Tool path in the cutting mode or tapping mode

Fig. 5.4.1 Example of Tool Paths from Block (1) to Block (2)

CAUTION

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

B–63514EN/01

PROGRAMMING

5. FEED FUNCTIONS

5.4.2

Automatic Corner Override

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

5.4.2.1

Automatic Override for Inner Corners (G62)

Explanations

D Override condition

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

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

xθxθpx178_ in Fig. 5.4.2.1 (a)

θp is a value set with parameter No. 1711. When θ is approximately

equal to

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

less.

:Tool :Programmed path :Cutter center path

3. Arc–straight line 4. Arc–arc

Fig. 5.4.2.1 (a) Inner corner

PROGRAMMING5. FEED FUNCTIONS

B–63514EN/01

Override range

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

Programmed path

Cutter center path

The feedrate is overridden from point a to point b.

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

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

Cutter center path

The feedrate is overridden from point a to b.

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

Programmed path

B–63514EN/01

PROGRAMMING

5. FEED FUNCTIONS

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

Programmed path

d a

LsLebLs Le

(2)

Override value

Limitations

D Acceleration/deceleratio

n before interpolation

D Start–up/G41, G42

D Offset

Tool

Cutter center path

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

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

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

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

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

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

PROGRAMMING5. FEED FUNCTIONS

B–63514EN/01

5.4.2.2

Internal Circular Cutting Feedrate Change

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

Rc : Cutter center path radius Rp : Programmed radius

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

Programmed path

Cutter center

Fig. 5.4.2.2 Internal circular cutting feedrate change

path

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

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

NOTE

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

(override for the inner corners)×(feedrate override)

B–63514EN/01

PROGRAMMING

5. FEED FUNCTIONS

5.4.3

Automatic Corner Deceleration

5.4.3.1

Corner Deceleration According to the Corner Angle

Explanations

D Flowchart for feedrate

control

This function automatically controls the feedrate at a corner according to the corner angle between the machining blocks or the feedrate difference between the blocks along each axis. This function is effective when ACD, bit 6 of parameter No. 1601, is set to 1, the system is in G64 mode (machining mode), and a cutting–feed block (block A) is followed by another cutting–feed block (block B). The feedrate between machining blocks is controlled according to the corner angle between the blocks or the feedrate difference between the blocks along each axis. These two methods can be switched with CSD, bit 4 of parameter No. 1602.

This function decelerates the feedrate when the angle between blocks A and B on the selected plane is smaller than the angle specified in parameter No. 1740. The function executes block B when the feedrates along both the first and second axes are smaller than the feedrate specified in parameter No. 1741. In this case, the function determines that the number of accumulated pulses is zero.

The flowchart for feedrate control is shown below.

START

Is the corner angle smaller than the angle specified in parameter (No. 1740)?

Yes

Are the feedrates along the X– and Y–axes smaller than that specified in parameter (No. 1741)?

Yes

The number of accumulated pulses is determined to be zero and block B is executed

END

Further decelerates the feedrate in block A

PROGRAMMING5. FEED FUNCTIONS

B–63514EN/01

D Feedrate and time

D Angle between two

blocks

1. Between linear movements

When the corner angle is smaller than the angle specified in the parameter, the relationship between the feedrate and time is as shown below. Although accumulated pulses equivalent to the hatched area remain at time t, the next block is executed because the feedrate of the automatic acceleration/deceleration circuit is smaller than the parameter–set value. This function is effective only for movement on the selected plane.

Feedrate V

Block A

Parameter–set feedrate

Block B

The angle between two blocks (blocks A and B) is assumed to be angle

θ, as shown below.

2. Between linear and circular movements (angle between the linear movement and tangent to the circular movement)

3. Between circular movements (angle between the tangents to the circular movements)

Time t

D Selected plane

D Corner roundness

The machining angle is compared with the angle specified in parameter (No. 1740) for movements on the selected plane only. Machining feedrates are compared with that specified in parameter (No. 1741) for movement along the first and second axes on the selected plane only. This means, when movement occurs along three or more axes, only that movement along the first and second axes on the selected plane is considered.

Corner roundness is determined by the angle and feedrate specified in parameter (Nos. 1740 and 1741). To always make a sharp corner, set the angle to zero and the feedrate to 180000 (equivalent to 180 degrees).

D Exact stop

Limitations

When G90 (exact stop) is specified, exact stop is performed irrespective of the angle and feedrate specified in parameter (Nos. 1740 and 1741).

This function cannot be enabled for a single block or during dry run.

B–63514EN/01

PROGRAMMING

5. FEED FUNCTIONS

5.4.3.2

Corner Deceleration According to the Feedrate Difference between Blocks Along Each Axis

Explanations

D Flowchart for feedrate

control

This function decelerates the feedrate when the difference between the feedrates at the end point of block A and the start point of block B along each axis is larger than the value specified in parameter No. 1781. The function executes block B when the feedrates along all axes are smaller than the feedrate specified in parameter No. 1741. In this case, the function determines that the number of accumulated pulses is zero.

The flowchart for feedrate control is shown below.

START

Is the feedrate difference between blocks along each axis larger than the value specified in parameter (No. 1781)?

Yes

Are the feedrates along all axes smaller than that specified in parameter (No. 1741)?

Further decelerates the feedrate in block A

D Feedrate and time

Yes

The number of accumulated pulses is determined to be zero and block B is executed.

END

When the feedrate difference between blocks along each axis is larger than the value specified in parameter No. 1781, the relationship between the feedrate and time is as shown below. Although accumulated pulses equivalent to the hatched area remain at time t, the next block is executed because the feedrate of the automatic acceleration/deceleration circuit is smaller than the feedrate specified in parameter No. 1741.

Feedrate V

Block A

Block B

Parameter–set feedrate

Time t

PROGRAMMING5. FEED FUNCTIONS

B–63514EN/01

D Setting the allowable

feedrate difference along each axis

D Checking the feedrate

difference

D Exact stop

D Override

Limitations

The allowable feedrate difference can be specified for each axis in parameter No. 1783.

The feedrate difference is also checked during dry–run operation or during deceleration caused by an external signal, using feedrate commands specified in a program.

When G90 (exact stop) is specified, exact stop is performed irrespective of the parameter settings.

If an override is changed during operation, the feedrate difference will not be checked correctly.

This function is not effective for feed–per–rotation commands, address–F–with–one–digit commands, rigid tapping, and a single block.

B–63514EN/01

5.5

DWELL (G04)

Format

PROGRAMMING

Dwell G04 X_ ; or G04 P_ ;

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

5. FEED FUNCTIONS

Explanations

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

Table 5.5 (a) Command value range of the dwell time

(Command by X)

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 5.5 (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

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–63514EN/01

fanuc 0i-MA Operators Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

B-63514EN/01

SAFETY PRECAUTIONS

DEFINITION OF WARNING, CAUTION, AND NOTE

GENERAL W ARNINGS AND CAUTIONS

W ARNINGS AND CAUTIONS RELATED TO PROGRAMMING

W ARNINGS AND CAUTIONS RELATED TO HANDLING

W ARNINGS RELATED TO DAILY MAINTENANCE

Table of Contents

I. GENERAL

1. GENERAL

1.1 GENERAL FLOW OF OPERATION OF CNC MACHINE TOOL

1.2 NOTES ON READING THIS MANUAL

II. PROGRAMMING

1. GENERAL

1.3 PART DRAWING AND TOOL MOVEMENT

1.7 PROGRAM CONFIGURATION

1.8 TOOL FIGURE AND TOOL MOTION BY PROGRAM

PROGRAMMING2. CONTROLLED AXES

2.1 CONTROLLED AXES

2.2 AXIS NAME

2.3 INCREMENT SYSTEM

2.4 MAXIMUM STROKE

PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING4. INTERPOLATION FUNCTIONS

4.1 POSITIONING (G00)

4.2 SINGLE DIRECTION POSITIONING (G60)

LINEAR INTERPOLATION (G01)

CIRCULAR INTERPOLATION (G02, G03)

HELICAL INTERPOLATION (G02, G03)

CYLINDRICAL INTERPOLATION (G07.1)

THREAD CUTTING (G33)

SKIP FUNCTION (G31)

4.9 HIGH SPEED SKIP SIGNAL (G31)

PROGRAMMING5. FEED FUNCTIONS

GENERAL

RAPID TRAVERSE

CUTTING FEED

CUTTING FEEDRATE CONTROL

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

Automatic Corner Override

Automatic Override for Inner Corners (G62)

Internal Circular Cutting Feedrate Change

Automatic Corner Deceleration

Corner Deceleration According to the Corner Angle

Corner Deceleration According to the Feedrate Difference between Blocks Along Each Axis

DWELL (G04)

PROGRAMMING6. REFERENCE POSITION