fanuc 0i-PC Operators Manual

Download











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

The export of this product is subject to the authorization of the government of the country from where the product is exported.

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–8. . . . . . . . . . . . . . . . . . .

5. WARNINGS RELATED TO DAILY MAINTENANCE s–10. . . . . . . . . . . . . . . . . . . . . . .

s–1

SAFETY PRECAUTIONS

B–64154EN/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–64154EN/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. Once machining has started, keep well clear of the machine. Some machines move their table

at high speed, presenting a risk of injury to persons standing nearby.

7. 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.

8. 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–64154EN/01

WARNING

9. 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–64154EN/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 this 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. 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.

4. 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.

s–5

SAFETY PRECAUTIONS

WARNING

5. Special M codes

In principle, a block which includes any of the following M codes, which specify the execution of special functions, must not contain any other codes. When it is impossible to avoid specifying an M code together with another code in the same block, refer to the relevant description in the manual supplied by the machine–tool builder. Failure to follow the specified procedure may result in damage to the machine or injury to the user.

S Forming mode/forming mode cancel S Workpiece clamp/unclamp S Nibbling mode/nibbling mode cancel S Switching between punch mode and laser mode

6. Function involving a rotation axis

B–64154EN/01

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.

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.

9. Torque limit skip

Before attempting a torque limit skip, apply the torque limit. If a torque limit skip is specified without the torque limit actually being applied, a move command will be executed without performing a skip.

10.Programmable mirror image

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

11. 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–64154EN/01

12.Auto–repositioning

13.C–axis control

SAFETY PRECAUTIONS

If the amount of retraction or return for auto–repositioning is changed, and repositioning is repeated many times, grasping of the workpiece may fail, possibly causing damage to the machine. Be careful therefore, when changing the amount of retraction or return.

Before attempting to specify C–axis control, select a tool which supports the use of C–axis control. If C–axis control is applied while an incompatible tool is selected, C–axis rotation may cause damage to the metal die, magazine, and/or hitter.

s–7

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

WARNING

1. Manual operation

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

SAFETY PRECAUTIONS

B–64154EN/01

2. Manual reference position return

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

3. Manual numeric command

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

4. Manual handle feed

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

5. Disabled override

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

6. Origin/preset operation

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

s–8

B–64154EN/01

7. Workpiece coordinate system shift

8. Software operator ’s panel and menu switches

SAFETY PRECAUTIONS

WARNING

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.

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.

9. Manual intervention

If manual intervention is performed during programmed operation of the machine, the tool path may vary when the machine is restarted. Before restarting the machine after manual intervention, therefore, confirm the settings of the manual absolute switches, parameters, and absolute/incremental command mode.

10.Feed hold, override, and single block

The feed hold, feedrate override, and single block functions can be disabled using custom macro system variable #3004. Be careful when operating the machine in this case.

11. Dry run

Usually, a dry run is used to confirm the operation of the machine. During a dry run, the machine operates at dry run speed, which differs from the corresponding programmed feedrate. Note that the dry run speed may sometimes be higher than the programmed feed rate.

12.Cutter and tool nose radius compensation in MDI mode

Pay careful attention to a tool path specified by a command in MDI mode, because cutter or tool nose radius compensation is not applied. When a command is entered from the MDI to interrupt in automatic operation in cutter or tool nose radius compensation mode, pay particular attention to the tool path when automatic operation is subsequently resumed. Refer to the descriptions of the corresponding functions for details.

13.Program editing

If the machine is stopped, after which the machining program is edited (modification, insertion, or deletion), the machine may behave unexpectedly if machining is resumed under the control of that program. Basically , do not modify, insert, or delete commands from a machining program while it is in use.

14.Safety zone function

Setting an invalid safety zone may cause damage to the machine. Be careful when changing the safety zone.

s–9

SAFETY PRECAUTIONS

W ARNINGS RELATED TO DAILY MAINTENANCE

WARNING

1. Memory backup battery replacement

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.

B–64154EN/01

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 this manual for details of the battery replacement procedure.

s–10

B–64154EN/01

2. Absolute pulse coder battery replacement

SAFETY PRECAUTIONS

WARNING

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 this manual for details of the battery replacement procedure.

and

s–11

SAFETY PRECAUTIONS

WARNING

3. Fuse replacement

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).

B–64154EN/01

s–12

B–64154EN/01

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

I. GENERAL

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

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

1.2 CAUTIONS ON READING THIS MANUAL 7. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.3 CAUTIONS ON VARIOUS KINDS OF DATA 7. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

II. PROGRAMMING

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

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

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

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

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

1.3.2 Coordinate System on Part Drawing and Coordinate System Specified by

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

1.4 SELECTION OF TOOL USED FOR VARIOUS MACHINING – TOOL FUNCTION 19. . . . . . . . . .

1.5 COMMAND FOR MACHINE OPERATIONS – MISCELLANEOUS FUNCTION 20. . . . . . . . . . . .

1.6 PROGRAM CONFIGURATION 21. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7 TOOL FIGURE AND TOOL MOTION BY PROGRAM 24. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.8 TOOL MOVEMENT RANGE – STROKE 25. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

Incremental Commands 18. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2. CONTROLLED AXES 26. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1 CONTROLLED AXES 27. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.2 AXIS NAME 27. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3 INCREMENT SYSTEM 27. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4 MAXIMUM STROKE 28. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3. PREPARATORY FUNCTION (G FUNCTION) 29. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4. INTERPOLATION FUNCTIONS 32. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.1 POSITIONING (G00) 33. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.2 LINEAR INTERPOLATION (G01) 35. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.3 CIRCULAR INTERPOLATION (G02, G03) 37. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.4 SKIP FUNCTION (G33) 41. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.5 HIGH SPEED SKIP SIGNAL (G33) 43. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.6 HELICAL INTERPOLATION (G02, G03) 44. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5. FEED FUNCTIONS 45. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.1 GENERAL 46. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.2 RAPID TRAVERSE 48. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.2.1 Rapid Traverse Rate by F Command 48. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–1

Table of Contents

5.2.2 Rapid Traverse Override 49. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.2.3 F1-digit (Programmable Rapid Traverse Override) 50. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–64154EN/01

5.3 CUTTING FEED 51. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4 CUTTING FEEDRATE CONTROL 53. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.1 Exact Stop (G09, G61) Cutting Mode (G64) 54. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.2 Automatic Corner Override 55. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.2.1 Inside–corner Override (G62) 55. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.2.2 Internal Circular Cutting Feedrate Change 57. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.3 Automatic Corner Deceleration 58. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.3.1 Corner deceleration according to the corner angle 58. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.3.2 Corner deceleration according to the feedrate difference between blocks along each axis 61. . . . .

5.5 DWELL (G04) 65. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6. REFERENCE POSITION 66. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.1 REFERENCE POSITION RETURN 67. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7. COORDINATE SYSTEM 70. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1 MACHINE COORDINATE SYSTEM 71. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2 WORKPIECE COORDINATE SYSTEM 72. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.1 Setting a Workpiece Coordinate System 72. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.2 Selecting a W orkpiece Coordinate System 73. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.3 Changing Workpiece Coordinate System 74. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.3 LOCAL COORDINATE SYSTEM 76. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.4 PLANE SELECTION 78. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8. COORDINATE VALUE AND DIMENSION 79. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1 ABSOLUTE AND INCREMENTAL PROGRAMMING (G90, G91) 80. . . . . . . . . . . . . . . . . . . . . . .

8.2 INCH/METRIC CONVERSION (G20,G21) 81. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3 DECIMAL POINT PROGRAMMING 82. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9. PRESSING FUNCTION 83. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1 PUNCH FUNCTION (1-CYCLE PRESSING) 84. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.1 Block in which Punching is Made 84. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2 POSITIONING & PRESSING OFF (G70) 86. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3 NIBBLING FUNCTION 87. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3.1 Circular Nibbling (G68) 89. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3.2 Linear Nibbling (G69) 93. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3.3 Notes on Circular Nibbling (G68) and Linear Nibbling (G69) 95. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4 NIBBLING BY M FUNCTION 97. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4.1 G00 Command in Nibbling Mode 98. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4.2 G01, G02, and G03 Commands in Nibbling Mode 99. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4.3 Notes on Nibbling by M Function 102. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5 EXTERNAL MOTION FUNCTION 103. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.S FUNCTION 104. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.1 SPECIFYING THE S CODE WITH A BINARY CODE 105. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.TOOL FUNCTION (T FUNCTION) 106. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–2

B–64154EN/01

Table of Contents

11.1 TOOL SELECTION FUNCTION 107. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2 T COMMAND NEGLECT 109. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3 TOOL OFFSET 110. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4 CONTROLLING THE TURRET-AXIS (T-AXIS) 111. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5 TOOL LIFE MANAGEMENT FUNCTION 112. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5.1 T ool Life Management Data 112. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5.2 Register and Change of T ool Life Management Data 112. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5.3 T ool Life 112. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.AUXILIARY FUNCTION 113. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.1 AUXILIARY FUNCTION (M FUNCTION) 114. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.2 MULTIPLE M COMMANDS IN A SINGLE BLOCK 116. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.3 THE SECOND AUXILIARY FUNCTIONS (B CODES) 117. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.PROGRAM CONFIGURATION 118. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1 PROGRAM COMPONENTS OTHER THAN PROGRAM SECTIONS 120. . . . . . . . . . . . . . . . . . . . .

13.2 PROGRAM SECTION CONFIGURATION 123. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.3 SUBPROGRAM (M98, M99) 129. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.FUNCTIONS TO SIMPLIFY PROGRAMMING 132. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1 PATTERN FUNCTION 133. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.1 Base Point Command (G72) 134. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.2 Bolt Hole Circle (G26) 135. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.3 Line at Angle (G76) 137. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.4 Arc (G77) 138. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.5 Grid (G78, G79) 139. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.6 Share Proofs (G86) 141. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.7 Square (G87) 143. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.8 Radius (G88) 144. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.9 Cut at Angle (G89) 145. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.10 Incremental Command Just After Pattern Function 146. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1.11 Notes on Pattern Functions 149. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2 MEMORY AND CALL BY A/B MACRO 150. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3 AUTOMATIC REPOSITIONING (G75) 151. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4 MACRO FUNCTION 157. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4.1 Storage of Macros 157. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4.2 Macro Call 158. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4.3 Nesting Call of Macros 159. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4.4 Macro Storage Capacity 160. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4.5 Storage and Call of Multiple Macros (Macro Numbers 90 to 99) 161. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4.6 Deletion of Stored Macros 161. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5 MULTI–PIECE MACHINING FUNCTION 162. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.1 Base Point Command of Multi-Piece Machining (G98) 162. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.2 Multi–Piece Machining Commands (G73, G74) 165. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.3 Setting of Machining Method for Multi–Piece Machining 166. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5.4 Command for Restarting Machining Multiple Products 167. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.6 BENDING COMPENSATION (G38, G39) 169. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.COMPENSATION FUNCTION 171. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1 OVERVIEW OF CUTTER COMPENSATION C (G40 TO G42) 172. . . . . . . . . . . . . . . . . . . . . . . . . . .

c–3

Table of Contents

B–64154EN/01

15.2 DETAILS OF CUTTER COMPENSATION C 178. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.1 General 178. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.2 T ool Movement in Start–up 179. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.3 T ool Movement in Of fset Mode 183. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.4 T ool Movement in Of fset Mode Cancel 197. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.5 Interference Check 203. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.6 Overcutting by Cutter Compensation 208. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.7 Input Command from MDI 209. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.8 G53 and G28 Commands in Cutter Compensation C Mode 210. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.3 TOOL COMPENSATION VALUES, NUMBER OF COMPENSATION VALUES,

AND ENTERING VALUES FROM THE PROGRAM (G10) 218. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.4 SCALING (G50, G51) 219. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.5 COORDINATE SYSTEM ROTATION (G84, G85) 224. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.6 NORMAL DIRECTION CONTROL (G40.1, G41.1, G42.1 OR G150, G151, G152) 230. . . . . . . . . . .

16.CUSTOM MACRO 236. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.1 VARIABLES 237. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.2 SYSTEM VARIABLES 241. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.3 ARITHMETIC AND LOGIC OPERATION 248. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.4 MACRO STATEMENTS AND NC STATEMENTS 253. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5 BRANCH AND REPETITION 254. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5.1 Unconditional Branch (GOTO Statement) 254. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5.2 Conditional Branch (IF Statement) 254. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5.3 Repetition (While Statement) 255. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6 MACRO CALL 258. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.1 Simple Call (G65) 258. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.2 Modal Call (G66) 263. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.3 Macro Call Using G Code 265. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.4 Macro Call Using an M Code 266. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.5 Subprogram Call Using an M Code 267. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.6 Subprogram Calls Using a T Code 268. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.7 Sample Program 269. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.7 PROCESSING MACRO STATEMENTS 271. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.7.1 Details of NC Statements and Macro Statements Execution 271. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.7.2 Caution for Using System V ariables 273. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.8 REGISTERING CUSTOM MACRO PROGRAMS 275. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.9 LIMITATIONS 276. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.10 EXTERNAL OUTPUT COMMANDS 277. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.11 INTERRUPTION TYPE CUSTOM MACRO 281. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.11.1 Specification Method 282. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.11.2 Details of Functions 283. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

17.PROGRAMMABLE DATA ENTRY (G10) 290. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

17.1 PROGRAMMABLE PARAMETER ENTRY 291. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

17.2 TOOL DATA ENTRY 293. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.AXIS CONTROL FUNCTIONS 294. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.1 ROTARY AXIS ROLL–OVER 295. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.2 C AXIS CONTROL (DIE ANGLE INDEXING) 296. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.2.1 Simultaneously Controlled Axes 297. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–4

B–64154EN/01

18.2.2 Increment System 297. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.2.3 Maximum Programmable Dimension 297. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.2.4 Automatic Acceleration/Deceleration 297. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.2.5 Manual Continuous Feed, Incremental Feed, Manual Reference Point Return 297. . . . . . . . . . . . . . . . . . .

18.2.6 Relationship with Absolute/Incremental Command (G90/G91) 297. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.2.7 Positioning in Smaller Angle Rotating Direction 297. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.2.8 Blocks Where C–axis Command is Possible 298. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.2.9 C–axis Command and its Operation 299. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.2.10 Pattern Function, Nibbling Function and C–axis Command 300. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.2.11 C–axis Command in Nibbling Mode 301. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.2.12 T–axis Command Ignore Signal TNG and C–axis Command 301. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.2.13 Compensating the Position of the C–axis 301. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.2.14 Compensating Backlash Along the C–axis for Each T ool Group 301. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Table of Contents

18.3 SIMPLE SYNCHRONOUS CONTROL 302. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

18.4 TANDEM CONTROL 305. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19.HIGH SPEED CUTTING FUNCTIONS 306. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19.1 FEEDRATE CLAMPING BY ARC RADIUS 307. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

19.2 ADVANCED PREVIEW CONTROL (G08) 308. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

III. OPERATION

1. GENERAL 313. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.1 MANUAL OPERATION 314. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.2 TOOL MOVEMENT BY PROGRAMMING–AUTOMATIC OPERATION 316. . . . . . . . . . . . . . . . . .

1.3 AUTOMATIC OPERATION 317. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4 TESTING A PROGRAM 319. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4.1 Check by Running the Machine 319. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4.2 How to View the Position Display Change without Running the Machine 320. . . . . . . . . . . . . . . . . . . . . .

1.5 EDITING A PART PROGRAM 321. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.6 DISPLAYING AND SETTING DATA 322. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7 DISPLAY 325. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.1 Program Display 325. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.2 Current Position Display 326. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.3 Alarm Display 326. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.4 Parts Count Display, Run Time Display 327. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.5 Graphic Display 327. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.8 DATA OUTPUT 328. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2. OPERATIONAL DEVICES 329. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1 SETTING AND DISPLAY UNITS 330. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.1 7.2″ Monochrome/8.4″ Color LCD/MDI Unit (Horizontal T ype) 331. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.2 7.2″ Monochrome/8.4″ Color LCD/MDI Unit (Vertical T ype) 332. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.3 Key Location of MDI (Horizontal T ype LCD/MDI Unit) 333. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1.4 Key Location of MDI (V ertical Type LCD/MDI Unit) 334. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.2 EXPLANATION OF THE KEYBOARD 335. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3 FUNCTION KEYS AND SOFT KEYS 337. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.1 General Screen Operations 337. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.2 Function Keys 338. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.3 Soft Keys 339. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.4 Key Input and Input Buffer 355. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–5

Table of Contents

2.3.5 W arning Messages 356. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.6 Soft Key Configuration 357. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–64154EN/01

2.4 EXTERNAL I/O DEVICES 358. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.1 F ANUC Handy File 360. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.2 F ANUC Floppy Cassette 360. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.3 F ANUC FA Card 361. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.4 F ANUC PPR 361. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.5 Portable T ape Reader 362. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5 POWER ON/OFF 363. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.1 Turning on the Power 363. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.2 Screen Displayed at Power–on 364. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.5.3 Power Disconnection 365. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3. MANUAL OPERATION 366. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.1 MANUAL REFERENCE POSITION RETURN 367. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.2 JOG FEED (JOG) 369. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.3 INCREMENTAL FEED 371. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.4 MANUAL HANDLE FEED 372. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.5 MANUAL ABSOLUTE ON 375. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4. AUT OMATIC OPERATION 379. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.1 MEMORY OPERATION 380. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.2 MDI OPERATION 383. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.3 DNC OPERATION 387. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.4 SCHEDULING FUNCTION 390. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.5 SUBPROGRAM CALL FUNCTION 395. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.6 MANUAL HANDLE INTERRUPTION 397. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.7 MIRROR IMAGE 400. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8 DNC OPERATION WITH MEMORY CARD 402. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8.1 Specification 402. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8.2 Operations 403. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8.2.1 DNC Operation 403. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8.2.2 Subprogram call (M198) 404. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8.3 Limitation and Notes 405. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8.4 Parameter 405. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8.5 Connecting PCMCIA Card Attachment 406. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8.5.1 Specification number 406. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8.5.2 Assembling 406. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.8.6 Recommended Memory Card 408. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5. TEST OPERATION 409. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.1 MACHINE LOCK AND AUXILIARY FUNCTION LOCK 410. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.2 FEEDRATE OVERRIDE 412. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.3 RAPID TRAVERSE OVERRIDE 413. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4 DRY RUN 415. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.5 SINGLE BLOCK 416. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.6 TOOL SELECTION 418. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.7 PUNCH 419. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–6

B–64154EN/01

Table of Contents

5.8 MANUAL PUNCH 420. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6. SAFETY FUNCTIONS 421. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.1 EMERGENCY STOP 422. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.2 OVERTRAVEL 423. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.3 STORED STROKE CHECK 424. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.4 STROKE CHECK BEFORE MOVEMENT 427. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.5 SAFETY ZONE CHECK 428. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.5.1 Punch Forbidden Area and Approach Forbidden Area (Type A) 429. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.5.2 Punch Forbidden Area and Approach Forbidden Area (T ype B) 430. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.5.3 Setting the Safety Zone 431. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.5.4 Setting the T ool Shape Area 432. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.5.5 Automatic Setting of the Safety Zone 433. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.5.6 Displaying the Safety Zones and T ool Zone 435. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7. ALARM AND SELF–DIAGNOSIS FUNCTIONS 436. . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1 ALARM DISPLAY 437. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2 ALARM HISTORY DISPLAY 439. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.3 CHECKING BY SELF–DIAGNOSTIC SCREEN 440. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8. DATA INPUT/OUTPUT 443. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1 FILES 444. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2 FILE SEARCH 446. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3 FILE DELETION 447. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4 PROGRAM INPUT/OUTPUT 448. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.1 Inputting a Program 448. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.2 Outputting a Program 451. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5 OFFSET DATA INPUT AND OUTPUT 453. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5.1 Inputting Offset Data 453. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5.2 Outputting Offset Data 454. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6 INPUTTING AND OUTPUTTING PARAMETERS AND

PITCH ERROR COMPENSATION DATA 455. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.1 Inputting Parameters 455. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.2 Outputting Parameters 456. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.3 Inputting Pitch Error Compensation Data 457. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.4 Outputting Pitch Error Compensation Data 458. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.7 INPUTTING/ OUTPUTTING CUSTOM MACRO COMMON VARIABLES 459. . . . . . . . . . . . . . . . .

8.7.1 Inputting Custom Macro Common Variables 459. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.7.2 Outputting Custom Macro Common Variable 460. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8 DISPLAYING DIRECTORY OF FLOPPY DISK 461. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.1 Displaying the Directory 462. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.2 Reading Files 465. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.3 Outputting Programs 466. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.8.4 Deleting Files 467. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.9 INPUTTING/OUTPUTTING TOOL DATA 469. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.9.1 Inputting Tool Data 469. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.9.2 Outputting T ool Data 470. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.10 OUTPUTTING A PROGRAM LIST FOR A SPECIFIED GROUP 472. . . . . . . . . . . . . . . . . . . . . . . . .

8.11 DATA INPUT/OUTPUT ON THE ALL IO SCREEN 473. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.11.1 Setting Input/Output–Related Parameters 474. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–7

Table of Contents

8.11.2 Inputting and Outputting Programs 475. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.11.3 Inputting and Outputting Parameters 480. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.11.4 Inputting and Outputting Offset Data 482. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.11.5 Outputting Custom Macro Common Variables 484. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.11.6 Inputting and Outputting Floppy Files 485. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–64154EN/01

8.12 DATA INPUT/OUTPUT USING A MEMORY CARD 490. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9. EDITING PROGRAMS 502. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1 INSERTING, ALTERING AND DELETING A WORD 503. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.1 W ord Search 504. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.2 Heading a Program 506. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.3 Inserting a W ord 507. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.4 Altering a W ord 508. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.5 Deleting a W ord 509. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2 DELETING BLOCKS 510. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.1 Deleting a Block 510. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.2 Deleting Multiple Blocks 511. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3 PROGRAM NUMBER SEARCH 512. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4 SEQUENCE NUMBER SEARCH 513. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5 DELETING PROGRAMS 515. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.1 Deleting One Program 515. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.2 Deleting All Programs 515. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.3 Deleting More Than One Program by Specifying a Range 516. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6 EDITING OF CUSTOM MACROS 517. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.7 BACKGROUND EDITING 518. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.8 PASSWORD FUNCTION 519. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.9 EXTENDED PART PROGRAM EDITING FUNCTION 521. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.9.1 Copying an Entire Program 522. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.9.2 Copying Part of a Program 523. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.9.3 Moving Part of a Program 524. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.9.4 Merging a Program 525. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.9.5 Supplementary Explanation for Copying,Moving and Merging 526. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.9.6 Replacement of W ords and Addresses 527. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.CREATING PROGRAMS 529. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.1 CREATING PROGRAMS USING THE MDI PANEL 530. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2 AUTOMATIC INSERTION OF SEQUENCE NUMBERS 531. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.3 CONVERSATIONAL PROGRAMMING WITH GRAPHIC FUNCTION 533. . . . . . . . . . . . . . . . . . . .

1 1.SETTING AND DISPLA YING DATA 537. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1 SCREENS DISPLAYED BY FUNCTION KEY

11.1.1 Position Display in the Work Coordinate System 546. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.2 Position Display in the Relative Coordinate System 547. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.3 Overall Position Display 549. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.4 Presetting the W orkpiece Coordinate System 550. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.5 Actual Feedrate Display 551. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.6 Display of Run Time and Parts Count 552. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.7 Operating Monitor Display 553. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–8

POS

545. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–64154EN/01

Table of Contents

11.2 SCREENS DISPLAYED BY FUNCTION KEY

PROG

(IN MEMORY MODE OR MDI MODE) 554. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.1 Program Contents Display Screen 555. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.2 Current Block Display Screen 556. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.3 Next Block Display Screen 557. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.4 Program Check Screen 558. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.5 Program Screen for MDI Operation 560. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3 SCREENS DISPLAYED BY FUNCTION KEY

11.3.1 Displaying Memory Used and a List of Programs 561. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3.2 Displaying a Program List for a Specified Group 564. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4 SCREENS DISPLAYED BY FUNCTION KEY

11.4.1 Setting and Displaying the Tool Offset Value 568. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.2 Displaying and Entering Setting Data 570. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.3 Displaying and Setting Items on the T ool Registration Screens 572. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.3.1 Displaying and setting items on the initial tool registration screen 572. . . . . . . . . . . . . . . . . . . . . .

11.4.3.2 Displaying and setting items on the tool number registration screen 574. . . . . . . . . . . . . . . . . . . . .

11.4.3.3 Displaying and setting items on the screen

for entering the numbers of tools used for replacement 576. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.3.4 Displaying and setting items on the screen for the number of press operations 577. . . . . . . . . . . . .

11.4.3.5 Displaying and setting items on the tool figure registration screen (for drawing figures) 578. . . . .

11.4.4 Displaying and Setting Items on the Safety Zone Setting Screen 580. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.5 Sequence Number Comparison and Stop 582. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.6 Displaying and Setting Run Time, Parts Count, and Time 584. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.7 Displaying and Setting the W orkpiece Origin Offset Value 586. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.8 Input of Measured W orkpiece Origin Of fsets 587. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.9 Displaying and Setting Custom Macro Common V ariables 589. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.10 Displaying and Setting the Software Operator’s Panel 590. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

PROG

(IN THE EDIT MODE) 561. . . . . . . . . . . . . . .

OFFSET SETTING

567. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5 SCREENS DISPLAYED BY FUNCTION KEY

SYSTEM

11.5.1 Displaying and Setting Parameters 593. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5.2 Displaying and Setting Pitch Error Compensation Data 595. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

AND WARNING MESSAGES FOR DATA SETTING OR INPUT/OUTPUT OPERATION 597. . . . .

11.6.1 Displaying the Program Number and Sequence Number 597. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.6.2 Displaying the Status and W arning for Data Setting or Input/Output Operation 598. . . . . . . . . . . . . . . . . .

11.7 SCREENS DISPLAYED BY FUNCTION KEY

MESSAGE

11.7.1 External Operator Message History Display 600. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8 CLEARING THE SCREEN 602. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8.1 Erase Screen Display 602. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.8.2 Automatic Erase Screen Display 603. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.GRAPHICS FUNCTION 604. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.1 OPERATION 605. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.2 REGISTERING THE TOOL FIGURE 606. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.3 SPECIFYING DRAWING PARAMETERS 607. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.4 GRAPHIC DISPLAY SCREEN AND DRAWING 612. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.5 EXAMPLE 615. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

592. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

c–9

Table of Contents

13.HELP FUNCTION 617. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

IV. MAINTENANCE

1. METHOD OF REPLACING BATTERY 625. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.1 REPLACING THE BATTERY FOR CONTROL UNIT 626. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.2 BATTERY FOR THE ABSOLUTE PULSE CODER 629. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.3 BATTERY FOR SEPARATE ABSOLUTE PULSE CODERS (6 VDC) 635. . . . . . . . . . . . . . . . . . . . . .

APPENDIX

A. TAPE CODE LIST 641. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B. LIST OF FUNCTIONS AND TAPE FORMAT 644. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

C. RANGE OF COMMAND VALUE 648. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D. NOMOGRAPHS 650. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D.1 TOOL PATH AT CORNER 651. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D.2 RADIUS DIRECTION ERROR AT CIRCLE CUTTING 654. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–64154EN/01

E. STATUS WHEN TURNING POWER ON,

WHEN CLEAR AND WHEN RESET 655. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

F. CHARACTER–TO–CODES CORRESPONDENCE TABLE 657. . . . . . . . . . . . . . . . . .

G. ALARM LIST 658. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

H. GLOSSARY 674. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–10

I. GENERAL

B–64154EN/01

GENERAL

About this manual

GENERAL

This manual consists of the following parts:

I. GENERAL

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

II. PROGRAMMING

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

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 procedure for replacing batteries.

APPENDIX

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

1. GENERAL

Special symbols

This manual does not describe parameters in detail. For details on parameters mentioned in this manual, refer to parameter manual (B–64160EN) of Series 0i–PC.

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–PC 0i–PC 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.

GENERAL1. GENERAL

B–64154EN/01

Related manuals

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

Manual name

FANUC Series 0i–MODEL C/0i Mate–MODEL C DESCRIPTIONS

FANUC Series 0i–MODEL C/0i Mate–MODEL C CONNECTION MANUAL (HARDWARE)

FANUC Series 0i–MODEL C/0i Mate–MODEL C CONNECTION MANUAL (FUNCTION)

FANUC Series 0i–PC CONNECTION MANUAL (FUNCTION)

FANUC Series 0i–PC OPERATOR’S MANUAL B–64154EN * FANUC Series 0i–MODEL C/0i Mate–MODEL C

MAINTENANCE MANUAL FANUC Series 0i–PC PARAMETER MANUAL B–64160EN Programming Macro Compiler/Macro Executor

PROGRAMMING MANUAL

Specification

number

B–64112EN

B–64113EN

B–64113EN–1

B–64153EN

B–64115EN

B–61803E–1

FANUC MACRO COMPILER (For Personal Computer) PROGRAMMING MANUAL

PMC PMC Ladder Language PROGRAMMING MANUAL B–61863E Network PROFIBUS–DP Board OPERA T OR’S MANUAL B–62924EN Ethernet Board/DA T A SERVER Board

OPERA T OR’S MANUAL FAST Ethernet Board/FAST DA TA SERVER

OPERA T OR’S MANUAL DeviceNet Board OPERA T OR’S MANUAL B–63404EN OPEN CNC FANUC OPEN CNC OPERATOR’S MANUAL

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

(DNC Operation Management Package)

B–66102E

B–63354EN

B–63644EN

B–62994EN

B–63214EN

B–64154EN/01

GENERAL

1. GENERAL

Related manuals of SERVO MOTOR ais/ ai series

Related manuals of SERVO MOTOR a series

The following table lists the manuals related to SERVO MOTOR ais/ ai series.

Manual name

FANUC AC SER VO MOTOR ais series FANUC AC SER VO MOTOR ai series DESCRIPTIONS

FANUC AC SER VO MOTOR ais series FANUC AC SER VO MOTOR ai series P ARAMETER MANUAL

FANUC AC SPINDLE MOT OR ai series DESCRIPTIONS

FANUC AC SPINDLE MOT OR ai series P ARAMETER MANUAL

FANUC SER VO AMPLIFIER ai series DESCRIPTIONS B–65282EN FANUC AC SER VO MOTOR ais series

FANUC AC SER VO MOTOR ai series FANUC AC SPINDLE MOT OR ai series MAINTENANCE MANUAL

Specification

number

B–65262EN

B–65270EN

B–65272EN

B–65280EN

B–65285EN

The following table lists the manuals related to SER VO MOTOR a series.

Manual name

Specification

number

FANUC AC SER VO MOTOR a series DESCRIPTIONS B–65142E FANUC AC SER VO MOTOR a series

P ARAMETER MANUAL FANUC AC SPINDLE MOT OR a series DESCRIPTIONS B–65152E FANUC AC SPINDLE MOT OR a series

P ARAMETER MANUAL FANUC SER VO AMPLIFIER a series DESCRIPTIONS B–65162E FANUC SER VO MOT OR a series

MAINTENANCE MANUAL

B–65150E

B–65160E

B–65165E

Either of the following servo motors and the corresponding spindle can be connected to the CNC covered in this manual.

– FANUC SERVO MOTOR ai series – FANUC SERVO MOTOR a series

This manual mainly assumes that the FANUC SER VO MOTOR ai series of servo motor is used. For servo motor and spindle information, refer to the manuals for the servo motor and spindle that are actually connected.

GENERAL1. GENERAL

B–64154EN/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 cutting process

4. Cutting tools and cutting conditions

Decide the cutting method in every cutting process.

B–64154EN/01

1.2

CAUTIONS ON READING THIS MANUAL

GENERAL

CAUTION

1 The function of an CNC machine tool system depends not

only on the CNC, but on the combination of the machine tool, its magnetic cabinet, the servo system, the CNC, the 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 This manual describes as many reasonable variations in

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

1. GENERAL

1.3

CAUTIONS ON V ARIOUS KINDS OF DATA

CAUTION

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

II. PROGRAMMING

B–64154EN/01

GENERAL

PROGRAMMING

1) Punching is performered after positioning.

............. Punching function

1. GENERAL

Punching

Tool T01 Tool T02

2) Continuous, repetitive punching can be performed without halting the pressing process after positioning

............. Nibbling function

3) By giving commands for block, it is possible to perform at multiple positions in a given profile.

............. Pattern function

Punching

Program command G00X––Y––T01 ; X––T02 ;

Program command M12 ; G01X––Q–– ; X––Y–– ; : : M13 ;

In case of line at angle (G76)

This CNC supports the eight different patterns that will be used most frequently.

Program command G76I––J––K–– ;

PROGRAMMING1. GENERAL

B–64154EN/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–64154EN/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

CAUTION

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

PROGRAMMING1. GENERAL

B–64154EN/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 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–64154EN/01

1.3

PART DRAWING AND TOOL MOVEMENT

PROGRAMMING

1. GENERAL

1.3.1

Reference Position (Machine–Specific Position)

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

Reference point

Distance between reference point and workpiece holder is intrinsically determined according to machines.

End locator

Workpiece holder

The distance between the reference point and the end locator is intrinsically determined according to machines.

Explanations

Fig. 1.3.1 Reference position

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

Reference position return is performed by manual button operation.

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

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

1.3.2

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

PROGRAMMING1. GENERAL

Program

B–64154EN/01

Explanations

D Coordinate system

Part drawing

Fig. 1.3.2 (a) Coordinate system

Coordinate system

CNC

Command

Tool

Workpiece

Machine tool

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–64154EN/01

PROGRAMMING

1. GENERAL

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

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

D Methods of setting the

two coordinate systems in the same position

When a workpiece is set on the table, these two coordinate systems lay as follows: 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 cut 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, when setting a workpiece to be machined to general turret punch press, the workpiece is held by the workpiece holders after positioning it by applying the end face of the workpiece to the end locator and workpiece holders mounted on the machine as illustrated below.

Face B

Workpiece

End locator

Workpiece holder

Face A

Generally , the distance between the reference point and the and locator as well as the distance between the reference point and the workpiece holders are intrinsically determined according to machines, and they are separated from each other by a fixed distance.

1.3.3

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

PROGRAMMING1. GENERAL

B–64154EN/01

Explanations

D Absolute coordinates

Coordinate values of command for moving the tool can be indicated by absolute or incremental designation (See II–8.1).

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

Command specifying movement from point A to point B

B(10,30,20)

G90 X10.0 Y30.0 Z20.0 ;

Coordinates of point B

Tool

D Incremental coordinates

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

Tool

X=40

Z=–10

Command specifying movement from point A to point B

Y=–30

G91 X40.0 Y–30.0 Z–10.0

Distance and direction for movement along each axis

;

B–64154EN/01

PROGRAMMING

1. GENERAL

1.4

SELECTION OF T OOL USED FOR VARIOUS MACHINING – TOOL FUNCTION

Examples

When drilling, tapping, 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

Turret

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

PROGRAMMING1. GENERAL

B–64154EN/01

1.5

COMMAND FOR MACHINE OPERA TIONS – MISCELLANEOUS FUNCTION

During machining, on–off operation of work holder and clamper is performed. For this purpose, on–off operations of workholder and clamper should be controlled.

Clamper

Work holder

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 and M code.

B–64154EN/01

PROGRAMMING

1. GENERAL

1.6

PROGRAM CONFIGURATION

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

Block

Tool movement sequence

Block

Program

Block

⋅ ⋅ ⋅ ⋅

Block

Fig. 1.6 (a) Program configuration

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

PROGRAMMING1. GENERAL

B–64154EN/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. 1.6 (b) Block configuration

Spindle function

Tool function

End of block

A block starts with a sequence number that identifies 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. 1.6 (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–64154EN/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

1.7

TOOL FIGURE AND TOOL MOTION BY PROGRAM

Explanations

PROGRAMMING1. GENERAL

B–64154EN/01

D Machining using the side

of cutter – Cutter compensation function (See II–15.1, 15.2)

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

Cutter path using cutter compensation

Machined part figure

Workpiece

Cutter

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

B–64154EN/01

PROGRAMMING

1. GENERAL

1.8

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

PROGRAMMING2. CONTROLLED AXES

CONTROLLED AXES

B–64154EN/01

2.1

CONTROLLED AXES

PROGRAMMING 2. CONTROLLED AXES

Item 0i–PC

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

2.2

AXIS NAME

Limitations

D Default axis name

D Duplicate axis names

2.3

INCREMENT SYSTEM

The names of the two basic axes are fixed to X and Y, while the names of additional axes can be set to any of A, B, C, U, V, W, and T. 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. If A, B, U, V and W is specified an axis name, the punch press macro function is not available.

Name of

increment

system

IS–A

IS–B

Least input

increment

0.01mm

0.001inch

0.01deg

0.001mm

0.0001inch

0.001deg

Least command

increment

0.01mm

0.001inch

0.01deg

0.001mm

0.0001inch

0.001deg

Maximum

stroke

999999.99mm

99999.999inch

999999.99deg

99999.999mm

9999.9999inch

99999.999deg

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–64154EN/01

2.4

MAXIMUM STROKE

Limitations

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

D T axis is the axis for turret indexing. D The least input increment is not provided for the turret axis. Neither

movement direction nor amount on the turret axis is commanded after address T, but the tool number is commanded. The control system moves the turret axis to the location being preset by a tool registering screen according to the specified tool number , and selects the specified tool.

B–64154EN/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)

Explanations

G01X ;

Y ; X ;

G00Y ;

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 as

indicated in Table 3.

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

power–up or reset.(3) For G22 and G23, G22 is set at power–up. 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 (G18) and bit

1 (G19) of parameter No. 3402.

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

3. When a G code not listed in the G code list is specified, or a G code

that has no corresponding option is specified, 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. G codes are indicated by group.

G01 is effective in this range.

3. PREPARATORY FUNCTION

01 00

00 02

00 07

(G FUNCTION)

G code

G00 G00 G01 G01 G02 G02 G03 G03 Circular interpolation (CCW) / Helical interpolation (CCW) G04 G04 G08 G08 G09 G09 Exact stop G10 G10 G11 G11

G17 G17 G18 G18 G19 G19 G20 G20 G21 G21 G22 G22

G23 G23 G26 G26 G28 G50 G32 G32 G33 G33 G38 G38 Bending compensation X G39 G39 Bending compensation Y G40 G40 G41 G41 G42 G42 Cutter compensation right

G40.1

(G150)

G41.1

(G151)

G42.1

(G152)

G50 G34 G51 G35 G52 G93 G53 G53 G54 G54 G55 G55 G56 G56 G57 G57 G58 G58 Work coordinates system 5 selection G59 G59 Work coordinates system 6 selection

G code Group Meaning

G40.1

(G150)

G41.1

(G151)

G42.1

(G152)

PROGRAMMING

T able 3 G code list (1/2)

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

Dwell Advanced preview control

Programmable data input Programmable data input mode cancel XpYp plane Where Xp : X–axis or an axis parallel to it ZpXp plane Y p : Y–axis or an axis parallel to it YpZp plane Zp : Z–axis or an axis parallel to it Input in inch Input in inch Stored stroke limit function on Stored stroke limit function off Bolt hole circle Automatic reference point return Automatic safety zone setting Skip function

Cutter compensation cancel Cutter compensation left

Normal direction control canceled

Left–side normal direction control turned on

Right–side normal direction control turned on Scaling on

Scaling off Local coordinate system setting Machine coordinate system selection Work coordinates system 1 selection Work coordinates system 2 selection Work coordinates system 3 selection Work coordinates system 4 selection

B–64154EN/01

15 12 00

PROGRAMMING

T able 3 G code list (2/2)

G code MeaningGroupG code

G61 G61 G62 G62 G64 G64 G65 G95 00 Custom macro simple call G66 G96 G67 G97 G68 G68 G69 G69 G70 G70 G72 G72 G73 G75 G74 G76 G75 G27 Automatic repositioning G76 G28 Line at angle G77 G29 Arc G78 G36 Grid I G79 G37 Grid II G84 G84 G85 G85 G86 G66 G87 G67 G88 G78 G89 G79 Cut at angle G90 G90 G91 G91 G92 G92 G98 G98

Exact stop mode Automatic corner override Continuous cutting mode

Custom macro modal call Custom macro modal call cancel Circular nibbling Linear nibbling Positioning & press off Standard point command Multi–piece machining command X Multi–piece machining command Y

Coorrdinate rotating on Coordinate rotating off Share proof Square Radius

Absolute command Incremental command Coordinate system setting Coordinate system setting (Multi–piece machining)

3. PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING4. INTERPOLATION FUNCTIONS

INTERPOLATION FUNCTIONS

B–64154EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.1

POSITIONING (G00)

Format

Explanations

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

G00 _;

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

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

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

D Nonlinear interpolation positioning

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

D Linear interpolation positioning

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

Start position

Linear interpolation positioning

End position

Non linear interpolation positioning

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

PROGRAMMING4. INTERPOLATION FUNCTIONS

B–64154EN/01

When G00X_Y_T ; is specified in a machine having a turret axis (T–axis), the X and Y axes move to the specified positions at rapid traverse rate and also the T–axis moves at the predetermined rapid traverse rate in such a way as to select a specified tool number. In a machine provided with a die angle index (C–axis), if “G00X_Y_ ; ” is specified, the X, Y, and C axes move simultaneously at the predetermined rapid traverse rate. Refer to “C axis control” for the details. Since this control system treats the turret punch press as a controlled system, the tool moves to the commanded position as fast as possible for punching as the basic principle. Accordingly, the tool is positioned at rapid traverse, punching is done after axis movement in the G00 mode, in principle. Refer to “Punch function” for details.

The rapid traverse rate in the G00 command is set for each axis independently by the machine tool builder (parameter No. 1420). Accordingly , the rapid traverse rate cannot be specified in the address F. In the positioning mode actuated by G00, the tool is accelerated to a predetermined speed at the start of a block and is decelerated at the end of a block. Execution proceeds to the next block after confirming the in–position.

“In–position” means that the feed motor is within the specified range. (This range is determined by the machine tool builder) (Parameter No.

1827)

CAUTION

For T– or C–axis command blocks, nonlinear interpolation positioning is performed, even if linear interpolation positioning is specified. And, for block including G28 or G53 command, nonlinear interpolation positioning is performed.

B–64154EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.2

LINEAR INTERPOLATION (G01)

Format

Explanations

Tools can move along a line

G01 _F_;

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

and for an incremental 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/min.

PROGRAMMING4. INTERPOLATION FUNCTIONS

B–64154EN/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)

Limitations

D Feedrate for the

rotation axis

(Start position)

200.00

X axis

D Punching (1–cycle pressing) is not performed in G01 mode. D T code can’t be specified in G01 mode. If specified, an alarm (No.

4600) occurs. However, when T code is specified independently and NMG (No. 16181#0) is set, an alarm does not occur.

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

(Start point)

90°

(End point)

Feedrate is 300 deg/min

B–64154EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.3

CIRCULAR INTERPOLATION (G02, G03)

Format

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

Arc in the XpYp plane

G17

Arc in the ZpXp plane

G18

Arc in the Y pZpplane

G19

G02 G03

Xp_Yp_

Xp_ p_

Yp_ Zp_

I_ J_ R_

I_ K_ R_

J_ K_

F_ ;

Table. 4.3 Description of the Command Format

Command Description

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

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

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

with sign R_ Arc radius with sign fixed to radius designation. F_ Feedrate along the arc

Explanations

PROGRAMMING4. INTERPOLATION FUNCTIONS

B–64154EN/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

G17

G03

G02

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

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

End point (x,y)

Center

Start point

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 value in a parameter (No.3410), an alarm (No.024) occurs.

B–64154EN/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 ;

(2)

r=50mm

Start point

End point

(1)

r=50mm

D Feedrate

Limitations

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 alarm (No.028)is displayed.

D Punching (1–cycle pressing) is not performed in G02 and G03 mode. D If T command is specified in G02 and G03 mode, however, when T

code is specified independently and NMG (No. 16181#0) is set, an alarm (No. 4600) doesn’t occur.

Examples

PROGRAMMING4. INTERPOLATION FUNCTIONS

100

B–64154EN/01

Y axis

50R

60 40

90 120 140

60R

200

The above tool path can be programmed as follows ; (1) In absolute programming

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

G92X200.0 Y40.0 ; 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–64154EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.4

SKIP FUNCTION (G33)

Format

Explanations

Linear interpolation can be commanded by specifying axial move following the G33 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. It is used also for measuring the dimensions of a workpiece.

G33 _ ; G33: 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 and #5062, as follows:

#5061 X axis coordinate value #5062 Y axis coordinate value

WARNING

Disable feedrate override, dry run, and automatic acceleration/deceleration (with parameter No. 6200 and subsequent parameters) when the feedrate per minute is specified, allowing for an error in the position of the tool when a skip signal is input.

NOTE

If G33 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 G33 command is specified.

Examples D The next block to G33 is

an incremental command

PROGRAMMING4. INTERPOLATION FUNCTIONS

G33 G91X100.0 F100;

Y50.0;

B–64154EN/01

Y50.0

D The next block to G33 is

an absolute command for 1 axis

Skip signal is input here

Fig. 4.4 (a) The next block is an incremental command

G33 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 G33 is

an absolute command for 2 axes

Actual motion

Motion without skip signal

Fig. 4.4 (b) The next block is an absolute command for 1 axis

G33 G90X200.0 F100;

X300.0 Y100.0;

Skip signal is input here

100

100 200 300

Fig. 4.4 (c) The next block is an absolute command for 2 axes

(300,100)

Actual motion

Motion without skip signal

B–64154EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.5

HIGH SPEED SKIP SIGNAL (G33)

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.

G33 IP_ ;

G33: One–shot G code (If is effective only in the block in which it is

specified)

4.6

HELICAL INTERPOLATION (G02, G03)

Format

PROGRAMMING4. INTERPOLATION FUNCTIONS

B–64154EN/01

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

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.

Restrictions

Tool path

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

D Cutter compensation is applied only for a circular arc. D T axis command and C axis command cannot be used in a block in

which a helical interpolation is commanded.

B–64154EN/01

FEED FUNCTIONS

PROGRAMMING

5. FEED FUNCTIONS

PROGRAMMING5. FEED FUNCTIONS

B–64154EN/01

5.1

GENERAL

D Feed functions

D Override

D Automatic acceleration/

deceleration

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

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

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

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

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

Rapid traverse rate

: Rapid traverse

rate

: Acceleration/

deceleration time constant for rapid traverse rate

Time

Feed rate

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

: Feedrate

: Acceleration/

deceleration time constant for a cutting feedrate

Time

B–64154EN/01

PROGRAMMING

5. FEED FUNCTIONS

D Tool path in a cutting

feed

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

Programmed path Actual tool path

Fig. 5.1 (b) Example of 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.

5.2

RAPID TRAVERSE

Format

PROGRAMMING5. FEED FUNCTIONS

G00 _ ;

G00 : G code (group 01) for positioning (rapid traverse)

_; Dimension word for the end point

B–64154EN/01

Explanations

5.2.1

Rapid T raverse Rate by F Command

The positioning command (G00) positions the tool by rapid traverse and punching is performed. 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: 25, 50, 75, 100%

Each axis rapid traverse rate of rapid traverse command (G00) are set independently to parameter by machine tool builders.

Whereas, by setting parameter G0F (No. 16050#0) to 1, the rapid traverse rate of X and Y axes to rapid traverse command (G00) can be designated by F code. Refer to the manual issued by a machine tool builder for this function.

There are following specifications notices for this function.

1) The feedrate specified by F code is the each axis rapid traverse rate of X and Y axes.

2) 4-step rapid traverse override can be applied to the rapid traverse rate designated by F code, using signals (ROV2, ROV1) from the machine side.

3) When axial move of rapid traverse (G00) is specified in the tape, memory and MDI modes, the rapid traverse rate may not specified by F code or when the speed command is 0, an alarm (No. 011) occurs.

4) In circular nibbling (G68), linear nibbling (G69) and nibbling by M function, the speed to nibbling pitch after the first punch point corresponds to the rapid traverse rate preset by the parameter (No.

1420).

5) F1-digit function for programmable rapid traverse override is ineffective.

6) When the rapid traverse rate designated by F code exceeds the speed preset by a parameter (set by a machine tool builder), it is clamped to the speed preset by the parameter (No. 1420).

B–64154EN/01

5.2.2

Rapid Traverse Override

PROGRAMMING

5. FEED FUNCTIONS

In the automatic operation, the rapid traverse override is applied to the rapid traverse rate by the switch on the machine operator’s panel or F1-digit command (See Subsection 5.2.3).

Either rapid traverse override being set by the switch on the machine operator’s panel or rapid traverse override being set by F1-digit command, whichever is lower, becomes effective.

Examples1

Examples2

One digit

F command

F1 100% 100% 100% F2 75% 75% 100% F3 50%

Rapid traverse override switch on

machine operator’s panel

25%

X-axis,

Y-axis

50% 25%

T-axis, C-axis

50% 50%

If F3 command is given when the switch on the machine operator’s panel is set to 100%, the rapid traverse override of the X and Y axes becomes 50%, and also that of T-axis and C axis becomes 50%.

If F1 command is given when the switch on the machine operator’s panel is set to 25%, the rapid traverse override of the X and Y axes becomes 25%, while that of T-axis and C axis becomes 50%.

In manual operation mode, the rapid traverse override by the switch on the machine operator’s panel and by one-digit F command is inef fective.

WARNING

For the T-axis and C axis, the rapid traverse override can always be set to 100% by setting a parameter TCO (No. 16052#1).

PROGRAMMING5. FEED FUNCTIONS

One-digit F command

B–64154EN/01

5.2.3

F1-digit (Programmable Rapid T raverse Override)

By specifying one-digit number from 1 to 4 following F , and override can be applied to the rapid traverse rate in automatic operation.

Rapid traverse override

X axis, Y axis T axis, C axis

F1 100% 100% F2 75% 100% F3 50% 50% F4 25% 50%

An override can be applied to the rapid traverse rate by the switch on the machine operator’s panel as well as by F1-digit command in automatic operation.

Either rapid traverse override being set by the switch or the rapid traverse override being set by F1-digit command, whichever lower, becomes effective (see 5.2.2) .

WARNING

1 For the T and C axis, the override can always be set to 100%

by setting a parameter TCO (No. 16052#1) . 2 F0 is equivalent to F1, while F5 to F9 are equivalent to F4. 3 When power is turned on, the machine is placed to the F1

command state.

If parameter CLR (No. 3402#6) is set to 1, this F1 state is

obtained after depressing the reset button. If CLR is set to

0, the state remains unchanged as before reset.

B–64154EN/01

PROGRAMMING

5. FEED FUNCTIONS

5.3

CUTTING FEED

Format

Explanations

D Tangential speed

constant control

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.

Feed per minute

F_ ; Feedrate command (mm/min or inch/min)

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

End point

Start point

D Feed per minute

Start point

Linear interpolation

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

Center

Circular interpolation

End point

The amount of feed of the tool per minute is to be directly specified by setting a number after F. An override from 0% to 254% (in 1% steps) can be applied to feed per minute with the switch on the machine operator’s panel. For detailed information, see the appropriate manual of the machine tool builder.

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

Tool

Workpiece

Table

Fig. 5.3 (b) Feed per minute

PROGRAMMING5. FEED FUNCTIONS

B–64154EN/01

WARNING

Cutting feed is invalid for the turret axis (T–axis) and C–axis.

T–axis and C–axis commands, therefore, cannot be

specified in linear interpolation (G01) mode and circular

interpolation (G02, G03) mode.

However, when the parameter CIP (No.16360#5) is set to

1, C–axis can be specified.

D Cutting feedrate clamp

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

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:

B–64154EN/01

Auto–

ic c

PROGRAMMING

5. FEED FUNCTIONS

5.4

CUTTING FEEDRATE CONTROL

Function name

Exact stop

Cutting mode

Automatic override for

mat

inner corners

Internal circular cutting feedrate change

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

T able 5.4 Cutting Feedrate Control

G code V alidity of G code Description

G09

G61

G64

G62

This function is valid for specified blocks only.

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

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

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

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

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.

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.

The internal circular cutting feedrate is changed.

Format

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). When parameter

NCI (No. 1601#5) is set tool, in–position check is not

executed. 2 Inner corner angle θ: 2°

< θ x α x 178°

(α is a set value)

Workpiece

Tool

Exact stop G09 _ ;

Cutting mode G64 ; Automatic corner override G62 ;

G61 ;

5.4.1

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

PROGRAMMING5. FEED FUNCTIONS

B–64154EN/01

Explanations

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

(2)

(1)

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

Position check Tool path in the exact stop mode

Tool path in the cutting mode

WARNING

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

clear.

B–64154EN/01

PROGRAMMING

5. FEED FUNCTIONS

5.4.2

Automatic Corner Override

This function enables producing a smooth cutting surface by decelerating tool movement automatically between an inside corner and an inside arc to reduce the load on the cutter during cutter compensation.

5.4.2.1

Inside–corner Override (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–64154EN/01

WARNING

When the block before a corner is a start–up block, or the

block after a corner includes G41 or G42, the feedrate is not

overridden. The feedrate override function is disabled when

the offset value is 0.

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

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)).

B–64154EN/01

PROGRAMMING

5. FEED FUNCTIONS

Programmed path

d a

LsLebLs Le

(2)

Override value

Restrictions

D Pre–interpolation

acceleration/deceleration

D Start–up or G41 and G42

D Offset data

5.4.2.2

Internal Circular Cutting Feedrate Change

Tool

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

Cutter center path

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)

The inside–corner override function is disabled during pre–interpolation acceleration/deceleration.

The inside–corner override function is disabled if a block before the corner is a start–up block for cutter compensation or a block after the corner contains G41 or G42.

The inside–corner override function is disabled if the offset data is 0.

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

PROGRAMMING5. FEED FUNCTIONS

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

WARNING

When internal circular cutting must be performed together

with automatic override for inner corners, the feedrate of the

tool is as follows:

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

(automatic override for the inner corners)

× (feedrate override)

B–64154EN/01

5.4.3

Automatic Corner Deceleration

5.4.3.1

Corner deceleration according to the corner angle

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.

B–64154EN/01

Explanations

PROGRAMMING

5. FEED FUNCTIONS

D Flowchart for feedrate

control

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

Further decelerates the feedrate in block A

D Feedrate and time

END

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

Time t

PROGRAMMING5. FEED FUNCTIONS

B–64154EN/01

D Acceleration/

deceleration before interpolation

D Angle between two

blocks

When acceleration/deceleration before interpolation is effective, the relationship between the feedrate and time is as shown below. When the angle between blocks A and B on the selected plane is smaller than the angle specified in parameter No. 1740, and the feedrates specified in blocks A and B are larger than that specified in parameter No. 1777, the feedrate is decelerated to the parameter–set value in block A, and accelerated to the feedrate specified in block B. The acceleration depends on the parameter for acceleration/deceleration before interpolation.

Feedrate

Block A

Parameter–set feedrate (parameter No. 1777)

Block B

Time

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

θ, as shown below.

1. Between linear movements

D Selected plane

D Corner roundness

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)

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

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

B–64154EN/01

PROGRAMMING

5. FEED FUNCTIONS

D Advanced preview

control

Limitations

5.4.3.2

Corner deceleration according to the feedrate difference between blocks along each axis

Those parameters related to automatic corner deceleration in advanced preview control mode are shown below.

Advanced

preview

control mode

Parameter description

Switching the methods for automatic corner deceleration

Lower limit of feedrate in automatic corner deceleration based on the angle

Limit angle in corner deceleration based on the angle

Normal

mode

1602#4 1602#4

1777 1778

1740 1779

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

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.

Explanations

D Flowchart for feedrate

control

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?

Yes

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

Further decelerates the feedrate in block A

END

PROGRAMMING5. FEED FUNCTIONS

B–64154EN/01

D Feedrate and time

D Acceleration /

deceleration before interpolation

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

Parameter–set feedrate

Block B

Time t

When acceleration/deceleration before interpolation is effective, the relationship between the feedrate and time is as described below. When the feedrate difference between blocks A and B along each axis is larger than the value specified in parameter No. 1780, the feedrate is decelerated to the corner feedrate calculated from the feedrate dif ference along each axis. Let the feedrate be F. Compare the feedrate difference along each axis (Vc[X], Vc[Y], ...) with the value specified in parameter No. 1780, Vmax. When the difference exceeds Vmax, calculate R as shown below.

Vmax

Find the maximum value for R among the calculated values for the axes. Let it be Rmax. Then, the corner feedrate can be obtained as follows:

Fc=F*

(Example)

Rmax

N1 G01 G91 X80. Y20. F3000 ; N2 X20. Y80. ;

When this movement is specified, the feedrate along each axis is as shown in the next figure.

Rmax=

Vc[X(Y)]

Vmax

Rmax

From the figure, it can be seen that the feedrate differences along the X– and Y–axes (Vc[X] and Vc[Y]) exceed Vmax. Calculate Rmax to get Fc. When the feedrate is decelerated to Fc at the corner, the feedrate difference along each axis do not exceed Vmax.

B–64154EN/01

PROGRAMMING

5. FEED FUNCTIONS

Without corner deceleration With corner deceleration

Feedrate along the X–axis

Feedrate along the Y–axis

Feedrate along the tangent at the corner

Rmax

Vc [X]

Vmax

Vc [Y]

D Setting the allowable

feedrate difference along each axis

D Checking the feedrate

difference

D Exact stop

D Override

N1 N2 t

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.

PROGRAMMING5. FEED FUNCTIONS

B–64154EN/01

D Advanced preview

control

Limitations

Parameters related to automatic corner deceleration in advanced preview control mode are shown below.

Advanced

preview

control mode

Parameter description

Switching the methods for automatic corner deceleration

Allowable feedrate difference (for all axis) in automatic corner deceleration based on the feedrate difference

Allowable feedrate difference (for each axis) in automatic corner deceleration based on the feedrate difference

Normal

mode

1602#4 ←

1780 ←

1783 ←

This function is not effective for a single block.

B–64154EN/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 (G62 mode). When neither P nor X is specified, exact stop is performed.

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

Increment system Command value range Dwell time unit

IS–A 0.01 to 999999.99 IS–B 0.001 to 99999.999

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

Increment system

IS–A 1 to 99999999 0.01 s IS–B 1 to 99999999 0.001 s

Command value range Dwell time unit

PROGRAMMING6. REFERENCE POSITION

REFERENCE POSITION

B–64154EN/01

6.1

REFERENCE POSITION RETURN

PROGRAMMING

6. REFERENCE POSITION

D Reference position

The reference position is a certain fixed point on the machine. It is defined as the point, to which a tool can be moved easily by the reference point return.

When setting a workpiece to be machined to general turret punch press, the workpiece is held by the workpiece holders after positioning it by applying the end face of the workpiece to the end locator and workpiece holders mounted on the machine as illustrated below.

Face B

End locator

Workpiece holder

Workpiece

Face A

Face B

Apply face B to the end locator.

End locator

Apply face A to workpiece holder.

Workpiece

Fig. 6.1 (a)

Face A

Workpiece holder

Generally , the distance between the reference position and the end locator as well as the distance between the reference position and the workpiece holders are intrinsically determined according to machines, and they are separated from each other by a fixed distance.

End locator

PROGRAMMING6. REFERENCE POSITION

Distance between reference position and workpiece holder is intrinsically determined according to machines.

Workpiece holder

The distance between the reference position and the end locator is intrinsically determined according to machines.

B–64154EN/01

Reference position

Fig. 6.1 (b)

Accordingly, if the start point is at the reference position and the point located at the left lower side of the workpiece is presumed as the zero point of the workpiece coordinate system, tool position at the start point can be taught to NC as a position in the workpiece coordinate system by giving the following command at the initial stage of programming.

G92X x

where, x

Y yR ;

: Distance from end locator to reference position along X-axis

: Distance from workpiece holder to reference position along

Y-axis

B–64154EN/01

PROGRAMMING

6. REFERENCE POSITION

D Reference position

return and movement from the reference position

Format

D Reference position

return

T ools are automatically moved to the reference position. When reference position return is completed, the lamp for indicating the completion of return goes on.

Reference position return A→R

R (Reference position)

A (Start position for reference position return)

Fig. 6.1 (c) Reference position return

G28_ ;

Reference position return

Explanations

D Reference position

return (G28)

Limitations D Status the machine lock

being turned on

D First return to the

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

D Lighting the lamp when

the programmed position does not coincide with the reference position

Reference positions are performed at the rapid traverse rate of each axis. When using this command, usually cancel the cutter compensation.

Example G28 M30;

The lamp for indicating the completion of return does not go on when the machine lock is turned on, even when the tool has automatically returned to the reference position.

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

When the machine tool system is an inch system with metric input, the reference position return lamp may also light up even if the programmed position is shifted from the reference position by 1

µ. This is because the

least input increment of the machine tool system is smaller than its least command increment.

Reference

D Manual reference

position return

See III–3.1.

PROGRAMMING7. COORDINATE SYSTEM

COORDINATE SYSTEM

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

X_Y_Z_

This command is referred to as a dimension word.

B–64154EN/01

25.0

50.0

40.0

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

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

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

B–64154EN/01

PROGRAMMING

7. COORDINATE SYSTEM

7.1

MACHINE COORDINATE SYSTEM

Format

Explanations

D Selecting a machine

coordinate system (G53)

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

G53 _ ;

_ : Absolute dimension word

When a command is specified based on a machine coordinate system, the tool moves by rapid traverse. G53, which is used to select a machine coordinate system, is a one–shot G code; that is, it is valid only in the block in which it is specified. The absolute command (G90) is valid. If the incremental command (G91) is specified, G53 is not executed. When the tool is to be moved to a machine–specific position such as a tool change position, program the movement in a machine coordinate system based on G53.

Limitations

D Cancel of the

compensation function

D G53 specification

immediately after power–on

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

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

PROGRAMMING7. COORDINATE SYSTEM

B–64154EN/01

7.2

WORKPIECE COORDINATE SYSTEM

7.2.1

Setting a Workpiece Coordinate System

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

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

(1) Method using G92

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

(2) Automatic setting

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

(3) Method using G54 to G59

After six workpiece coordinate systems are set from the MDI panel, the program commands G54 to G59 are used to select which workpiece coordinate system is used (see III–11.4.7). Before specifying the absolute command, use one of the above methods to establish the workpiece coordinate system.

Format

D Setting a workpiece

coordinate system by G92

Explanations

Examples

(G90) G92 _IP

A workpiece coordinate system is set so that a point on the tool, such as the tool tip, is at specified coordinates. Cutter compensation is cancelled temporarily with G92. M.S and T code cannot be specified in G92 block.

1016.0

Meet the programming start point with a center of the tool and command G92 at the start of program.

G92X1270.0Y1016.0 ;

1270.0

B–64154EN/01

PROGRAMMING

7. COORDINATE SYSTEM

7.2.2

Selecting a Workpiece Coordinate System

Examples

The user can choose from set workpiece coordinate systems as described below . (For information about the methods of setting, see Section 7.2.1.)

(1) Selecting a workpiece coordinate system set by G92 or automatic

workpiece coordinate system setting

Once a workpiece coordinate system is selected, absolute commands work with the workpiece coordinate system.

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

MDI panel

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

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

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

G90 G55 G00 X40.0 Y100.0 ;

Workpiece coordinate system 2 (G55)

100.0

40.0

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

Fig. 7.2.2

PROGRAMMING7. COORDINATE SYSTEM

B–64154EN/01

7.2.3

Changing Workpiece Coordinate System

The six workpiece coordinate systems specified with G54 to G59 can be changed by changing an external workpiece zero point offset value or workpiece zero point offset value. Three methods are available to change an external workpiece zero point offset value or workpiece zero point offset value. (1) Inputting from the MDI panel (see III–11.4.7) (2) Programming by G10 or G92 (3) Changing an external workpiece zero point offset value (refer to

Workpiece coordinate system 1 (G54)

ZOFS1

EXOFS

Machine zero

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

machine tool builder’s manual)

Workpiece coordinate system 2 (G55)

ZOFS2

Workpiece coordinate system 3 (G56)

ZOFS3

ZOFS4

ZOFS5

ZOFS6

Workpiece coordinate system 4 (G57)

Workpiece coordinate system 5 (G58)

Workpiece coordinate system 6 (G59)

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

Format

D Changing by G10

D Changing by G92

G10 L2 Pp _;

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

workpiece coordinate system 1 to 6

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

offset for each axis.

G92 _;IP

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

Explanations

D Changing by G10

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

B–64154EN/01

PROGRAMMING

7. COORDINATE SYSTEM

D Changing by G92

Examples

By specifying G92 IP_;, a workpiece coordinate system (selected with a code from G54 to G59) is shifted to set a new workpiece coordinate system so that the current tool position matches the specified coordinates ( IP_). Then, the amount of coordinate system shift is added to all the workpiece zero point offset values. This means that all the workpiece coordinate systems are shifted by the same amount.

WARNING

When a coordinate system is set with G92 after an external workpiece zero point offset value is set, the coordinate system is not affected by the external workpiece zero point offset value. When G92X100.0Y80.0; is specified, for example, the coordinate system having its current tool reference position at X = 100.0 and Y = 80.0 is set.

If G92X100Y100; is commanded when the tool is positioned at (200,

160) in G54 mode, workpiece coordinate system 1 (X’ – Y’) shifted by vector A is created.

160

100

YȀY

G54 workpiece coordinate system

Tool position

100

200

New workpiece

XȀ

coordinate system

Original workpiece

coordinate system

PROGRAMMING7. COORDINATE SYSTEM

B–64154EN/01

7.3

LOCAL COORDINATE SYSTEM

Format

Explanations

When a program is created in a workpiece coordinate system, a child workpiece coordinate system may be set for easier programming. Such a child coordinate system is referred to as a local coordinate system.

G52 _; Setting the local coordinate system

......

G52 0 ; Canceling of the local coordinate system

_ : Origin of the local coordinate system

By specifying G52 IP_;, a local coordinate system can be set in all the workpiece coordinate systems (G54 to G59). The origin of each local coordinate system is set at the position specified by IP_ in the workpiece coordinate system. When a local coordinate system is set, the move commands in absolute mode (G90), which is subsequently commanded, are the coordinate values in the local coordinate system. The local coordinate system can be changed by specifying the G52 command with the zero point of a new local coordinate system in the workpiece coordinate system. T o cancel the local coordinate system and specify the coordinate value in the workpiece coordinate system, match the zero point of the local coordinate system with that of the workpiece coordinate system.

Reference point

(Local coordinate system)

(G54 : Workpiece coordinate system 1)

G55

Machine coordinate system origin

Fig. 7.3 Setting the local coordinate system

G56

G57

G58

(Machine coordinate system)

(Local coordinate system)

(G59 : Workpiece coordinate system 6)

fanuc 0i-PC Operators Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

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

GENERAL

GENERAL FLOW OF OPERATION OF CNC MACHINE TOOL

CAUTIONS ON READING THIS MANUAL

CAUTIONS ON V ARIOUS KINDS OF DATA

II. PROGRAMMING

GENERAL

TOOL MOVEMENT ALONG WORKPIECE P ARTS FIGURE– INTERPOLATION

FEED– FEED FUNCTION

PART DRAWING AND TOOL MOVEMENT

Reference Position (Machine–Specific Position)

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

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

SELECTION OF T OOL USED FOR VARIOUS MACHINING – TOOL FUNCTION

COMMAND FOR MACHINE OPERA TIONS – MISCELLANEOUS FUNCTION

PROGRAM CONFIGURATION

TOOL FIGURE AND TOOL MOTION BY PROGRAM

TOOL MOVEMENT RANGE – STROKE

CONTROLLED AXES

CONTROLLED AXES

AXIS NAME

INCREMENT SYSTEM

MAXIMUM STROKE

PREPARATORY FUNCTION (G FUNCTION)

INTERPOLATION FUNCTIONS

POSITIONING (G00)

LINEAR INTERPOLATION (G01)

CIRCULAR INTERPOLATION (G02, G03)

SKIP FUNCTION (G33)

HIGH SPEED SKIP SIGNAL (G33)

HELICAL INTERPOLATION (G02, G03)

FEED FUNCTIONS

GENERAL

RAPID TRAVERSE

Rapid T raverse Rate by F Command

Rapid Traverse Override

F1-digit (Programmable Rapid T raverse Override)

CUTTING FEED

CUTTING FEEDRATE CONTROL

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

Automatic Corner Override

Inside–corner Override (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)

REFERENCE POSITION

REFERENCE POSITION RETURN

COORDINATE SYSTEM

MACHINE COORDINATE SYSTEM

WORKPIECE COORDINATE SYSTEM

Setting a Workpiece Coordinate System

Selecting a Workpiece Coordinate System

Changing Workpiece Coordinate System

LOCAL COORDINATE SYSTEM