GE Fanuc 0-MD, 0-GSD Operator's Manual

Download



   





 

SAFETY PRECAUTIONS

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

Contents

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

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

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

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

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

s–1

SAFETY PRECAUTIONS

B–62574EN/02

DEFINITION OF WARNING, CAUTION, AND NOTE

This manual includes safety precautions for protecting the user and preventing damage to the machine. Precautions are classified into W arning and Caution according to their bearing on safety. Also, supplementary information is described as a Note. Read the Warning, Caution, and Note thoroughly before attempting to use the machine.

WARNING

Applied when there is a danger of the user being injured or when there is a damage of both the user being injured and the equipment being damaged if the approved procedure is not observed.

CAUTION

Applied when there is a danger of the equipment being damaged, if the approved procedure is not observed.

NOTE

The Note is used to indicate supplementary information other than Warning and Caution.

 Read this manual carefully, and store it in a safe place.

s–2

B–62574EN/02

SAFETY PRECAUTIONS

GENERAL WARNINGS AND CAUTIONS

WARNING

Never attempt to machine a workpiece without first checking the operation of the machine. Before starting a production run, ensure that the machine is operating correctly by performing a trial run using, for example, the single block, feedrate override, or machine lock function or by operating the machine with neither a tool nor workpiece mounted. Failure to confirm the correct operation of the machine may result in the machine behaving unexpectedly, possibly causing damage to the workpiece and/or machine itself, or injury to the user.

Before operating the machine, thoroughly check the entered data. Operating the machine with incorrectly specified data may result in the machine behaving unexpectedly , possibly causing damage to the workpiece and/or machine itself, or injury to the user.

Ensure that the specified feedrate is appropriate for the intended operation. Generally , for each machine, there is a maximum allowable feedrate. The appropriate feedrate varies with the intended operation. Refer to the manual provided with the machine to determine the maximum allowable feedrate. If a machine is run at other than the correct speed, it may behave unexpectedly , possibly causing damage to the workpiece and/or machine itself, or injury to the user.

When using a tool compensation function, thoroughly check the direction and amount of compensation. Operating the machine with incorrectly specified data may result in the machine behaving unexpectedly , possibly causing damage to the workpiece and/or machine itself, or injury to the user.

The parameters for the CNC and PMC are factory–set. Usually , there is not need to change them. When, however, there is not alternative other than to change a parameter, ensure that you fully understand the function of the parameter before making any change. Failure to set a parameter correctly may result in the machine behaving unexpectedly , possibly causing damage to the workpiece and/or machine itself, or injury to the user.

Immediately after switching on the power, do not touch any of the keys on the MDI panel until the position display or alarm screen appears on the CNC unit. Some of the keys on the MDI panel are dedicated to maintenance or other special operations. Pressing any of these keys may place the CNC unit in other than its normal state. Starting the machine in this state may cause it to behave unexpectedly.

This 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–62574EN/02

W ARNING

Some functions may have been implemented at the request of the machine–tool builder. When using such functions, refer to the manual supplied by the machine–tool builder for details of their use and any related cautions.

NOTE

Programs, parameters, and macro variables are stored in nonvolatile memory in the CNC unit. Usually , they are retained even if the power is turned off. Such data may be deleted inadvertently, however, or it may prove necessary to delete all data from nonvolatile memory as part of error recovery. To guard against the occurrence of the above, and assure quick restoration of deleted data, backup all vital data, and keep the backup copy in a safe place.

s–4

B–62574EN/02

SAFETY PRECAUTIONS

WARNINGS AND CAUTIONS RELATED TO PROGRAMMING

This section covers the major safety precautions related to programming. Before attempting to perform programming, read the supplied this manual carefully such that you are fully familiar with their contents.

WARNING

Coordinate system setting

If a coordinate system is established incorrectly, the machine may behave unexpectedly as a result of the program issuing an otherwise valid move command. Such an unexpected operation may damage the tool, the machine itself, the workpiece, or cause injury to the user.

Positioning by nonlinear interpolation

When performing positioning by nonlinear interpolation (positioning by nonlinear movement between the start and end points), the tool path must be carefully confirmed before performing programming. Positioning involves rapid traverse. If the tool collides with the workpiece, it may damage the tool, the machine itself, the workpiece, or cause injury to the user.

Function involving a rotation axis

When programming polar coordinate interpolation or normal–direction (perpendicular) control, pay careful attention to the speed of the rotation axis. Incorrect programming may result in the rotation axis speed becoming excessively high, such that centrifugal force causes the chuck to lose its grip on the workpiece if the latter is not mounted securely. Such mishap is likely to damage the tool, the machine itself, the workpiece, or cause injury to the user.

Inch/metric conversion

Switching between inch and metric inputs does not convert the measurement units of data such as the workpiece origin offset, parameter, and current position. Before starting the machine, therefore, determine which measurement units are being used. Attempting to perform an operation with invalid data specified may damage the tool, the machine itself, the workpiece, or cause injury to the user.

Constant surface speed control

When an axis subject to constant surface speed control approaches the origin of the workpiece coordinate system, the spindle speed may become excessively high. Therefore, it is necessary to specify a maximum allowable speed. Specifying the maximum allowable speed incorrectly may damage the tool, the machine itself, the workpiece, or cause injury to the user.

s–5

SAFETY PRECAUTIONS

W ARNING

Stroke check

After switching on the power, perform a manual reference position return as required. Stroke check is not possible before manual reference position return is performed. Note that when stroke check is disabled, an alarm is not issued even if a stroke limit is exceeded, possibly damaging the tool, the machine itself, the workpiece, or causing injury to the user.

Tool post interference check

A tool post interference check is performed based on the tool data specified during automatic operation. If the tool specification does not match the tool actually being used, the interference check cannot be made correctly, possibly damaging the tool or the machine itself, or causing injury to the user. After switching on the power, or after selecting a tool post manually, always start automatic operation and specify the tool number of the tool to be used.

Absolute/incremental mode

B–62574EN/02

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

Plane selection

If an incorrect plane is specified for circular interpolation, helical interpolation, or a canned cycle, the machine may behave unexpectedly . Refer to the descriptions of the respective functions for details.

10.

Torque limit skip

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

11.

Programmable mirror image

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

12.

Compensation function

If a command based on the machine coordinate system or a reference position return command is issued in compensation function mode, compensation is temporarily canceled, resulting in the unexpected behavior of the machine. Before issuing any of the above commands, therefore, always cancel compensation function mode.

s–6

B–62574EN/02

SAFETY PRECAUTIONS

WARNINGS AND CAUTIONS RELATED TO HANDLING

This section presents safety precautions related to the handling of machine tools. Before attempting to operate your machine, read the supplied this manual carefully , such that you are fully familiar with their contents.

WARNING

Manual operation

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

Manual reference position return

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

Manual numeric command

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

Manual handle feed

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

Disabled override

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

Origin/preset operation

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

s–7

SAFETY PRECAUTIONS

W ARNING

Workpiece coordinate system shift

Manual intervention, machine lock, or mirror imaging may shift the workpiece coordinate system. Before attempting to operate the machine under the control of a program, confirm the coordinate system carefully. If the machine is operated under the control of a program without making allowances for any shift in the workpiece coordinate system, the machine may behave unexpectedly , possibly damaging the tool, the machine itself, the workpiece, or causing injury to the operator.

Software operator’s panel and menu switches

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

B–62574EN/02

Manual intervention

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

10.

Feed hold, override, and single block

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

11.

Dry run

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

12.

Cutter and tool nose radius compensation in MDI mode

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

13.

Program editing

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

s–8

B–62574EN/02

SAFETY PRECAUTIONS

WARNINGS RELATED TO DAILY MAINTENANCE

WARNING

Memory backup battery replacement

When replacing the memory backup batteries, keep the power to the machine (CNC) turned on, and apply an emergency stop to the machine. Because this work is performed with the power on and the cabinet open, only those personnel who have received approved safety and maintenance training may perform this work. When replacing the batteries, be careful not to touch the high–voltage circuits (marked fitted with an insulating cover). Touching the uncovered high–voltage circuits presents an extremely dangerous electric shock hazard.

and

NOTE

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

s–9

SAFETY PRECAUTIONS

B–62574EN/02

W ARNING

Absolute pulse coder battery replacement

NOTE

The absolute pulse coder uses batteries to preserve its absolute position. If the battery voltage drops, a low battery voltage alarm is displayed on the machine operator’s panel or CR T screen. When a low battery voltage alarm is displayed, replace the batteries within a week. Otherwise, the absolute position data held by the pulse coder will be lost. Refer to the maintenance section of this manual for details of the battery replacement procedure.

and

s–10

B–62574EN/02

SAFETY PRECAUTIONS

W ARNING

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).

s–1 1

B–62574EN/02

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

I GENERAL

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

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

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

II PROGRAMMING

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

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

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

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

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

1.3.2 Coordinate System on Part Drawing and Coordinate System Specified by

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

1.4 CUTTING SPEED – SPINDLE SPEED FUNCTION 21. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.5 SELECTION OF TOOL USED FOR VARIOUS MACHINING – TOOL FUNCTION 22. . . . . . . . . .

1.6 COMMAND FOR MACHINE OPERATIONS – MISCELLANEOUS FUNCTION 23. . . . . . . . . . . . .

1.7 PROGRAM CONFIGURATION 24. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.8 TOOL FIGURE AND TOOL MOTION BY PROGRAM 27. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.9 TOOL MOVEMENT RANGE – STROKE 28. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

2. CONTROLLED AXES 29. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1 CONTROLLED AXES 30. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.2 NAME OF AXES 30. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

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

3. REPARATORY FUNCTION (G FUNCTION) 31. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4. INTERPOLATION FUNCTIONS 34. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.1 POSITIONING (G00) 35. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.2 SINGLE DIRECTION POSITIONING (G60) 36. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.3 LINEAR INTERPOLATION (G01) 37. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.4 CIRCULAR INTERPOLATION (G02,G03) 39. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.5 SKIP FUNCTION (G31) (FOR 0–GSD ONLY) 43. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

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

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

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

5.3 CUTTING FEED 49. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4 CUTTING FEEDRATE CONTROL 51. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4.1 Exact Stop (G09, G61) Cutting Mode (G64) Tapping Mode (G63) 52. . . . . . . . . . . . . . . . . . . . . . . . . . .

c–1

Table of Contents

5.4.2 Internal Circular Cutting Feedrate Change 53. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–62574EN/02

5.5 DWELL (G04) 54. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6. REFERENCE POSITION 55. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7. COORDINATE SYSTEM 59. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1 MACHINE COORDINATE SYSTEM 60. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2 WORKPIECE COORDINATE SYSTEM 61. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.1 Setting a Workpiece Coordinate System 61. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.2 Selecting a Workpiece Coordinate System 62. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2.3 Changing Workpiece Coordinate System 63. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.3 LOCAL COORDINATE SYSTEM 65. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.4 PLANE SELECTION 67. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8. COORDINATE VALUE AND DIMENSION 68. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1 ABSOLUTE AND INCREMENTAL PROGRAMMING (G90, G91) 69. . . . . . . . . . . . . . . . . . . . . . . .

8.2 INCH/METRIC CONVERSION (G20,G21) 70. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3 DECIMAL POINT PROGRAMMING 71. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9. SPINDLE SPEED FUNCTION (S FUNCTION) 73. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1 SPECIFYING THE SPINDLE SPEED WITH A BINARY CODE 74. . . . . . . . . . . . . . . . . . . . . . . . . .

9.2 SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY (S5–DIGIT COMMAND) 74. . . . . . . . .

10.TOOL FUNCTION (T FUNCTION) 75. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.1 TOOL SELECTION FUNCTION 76. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.AUXILIARY FUNCTION 77. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1 AUXILIARY FUNCTION (M FUNCTION) 78. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2 MULTIPLE M COMMANDS IN A SINGLE BLOCK 79. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3 THE SECOND AUXILIARY FUNCTIONS (B CODES) (FOR 0–MD ONLY) 80. . . . . . . . . . . . . . . .

12.PROGRAM CONFIGURATION 81. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.1 PROGRAM COMPONENTS OTHER THAN PROGRAM SECTIONS 83. . . . . . . . . . . . . . . . . . . . . .

12.2 PROGRAM SECTION CONFIGURATION 86. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12.3 SUBPROGRAM 92. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.FUNCTIONS TO SIMPLIFY PROGRAMMING 96. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1 CANNED CYCLE 97. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.1 High–speed Peck Drilling Cycle (G73) 101. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.2 Left–handed Tapping Cycle (G74) 103. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.3 Fine Boring Cycle (G76) 105. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.4 Drilling Cycle, Spot Drilling (G81) 107. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.5 Drilling Cycle Counter Boring Cycle (G82) 109. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.6 Peck Drilling Cycle (G83) 111. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.7 Tapping Cycle (G84) 113. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.8 Boring Cycle (G85) 115. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.9 Boring Cycle (G86) 117. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.10 Boring Cycle Back Boring Cycle (G87) 119. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–2

B–62574EN/02

13.1.11 Boring Cycle (G88) 121. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.12 Boring Cycle (G89) 123. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.1.13 Canned Cycle Cancel (G80) 124. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Table of Contents

13.2 RIGID TAPPING 127. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.2.1 Rigid Tapping (G84) 127. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.2.2 Left–handed Rigid Tapping Cycle (G74) 129. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.2.3 Peck Rigid Tapping Cycle (G84 or G74) 131. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.2.4 Canned Cycle Cancel (G80) 132. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.3 CANNED GRINDING CYCLE (FOR 0–GSD ONLY) 133. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.3.1 Plunge Grinding Cycle (G75) 134. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.3.2 Direct Constant–dimension Plunge Grinding Cycle (G77) 136. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.3.3 Continuous–feed Surface Grinding Cycle (G78) 138. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.3.4 Intermittent–feed Surface Grinding Cycle (G79) 140. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.4 AUTOMATIC GRINDING WHEEL DIAMETER COMPENSATION AFTER DRESSING 142. . . . . .

13.4.1 Checking the Minimum Grinding Wheel Diameter (for 0–GSD only) 142. . . . . . . . . . . . . . . . . . . . . . . . .

13.5 IN–FEED GRINDING ALONG THE Y AND Z AXES AT THE END OF TABLE SWING

(FOR 0–GSD ONLY) 143. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13.6 EXTERNAL MOTION FUNCTION (G81) 144. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.COMPENSATION FUNCTION 145. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.1 TOOL LENGTH OFFSET (G43,G44,G49) 146. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.2 OVERVIEW OF CUTTER COMPENSATION C (G40 – G42) 150. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3 DETAILS OF CUTTER COMPENSATION C 156. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.1 General 156. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.2 Tool Movement in Start–up 157. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.3 Tool Movement in Offset Mode 161. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.4 Tool Movement in Offset Mode Cancel 175. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.5 Interference Check 181. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.6 Overcutting by Cutter Compensation 186. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.3.7 Input Command from MDI 189. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.4 TOOL COMPENSATION VALUES, NUMBER OF COMPENSATION VALUES,

AND ENTERING VALUES FROM THE PROGRAM (G10) 190. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

14.5 NORMAL DIRECTION CONTROL (G150, G151, G152) (FOR 0–GSD ONLY) 192. . . . . . . . . . . . . .

15.CUSTOM MACRO A 196. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1 CUSTOM MACRO COMMAND 197. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1.1 M98 (Single call) 197. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1.2 Subprogram call using M code 197. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1.3 Subprogram call using T code 198. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1.4 G66 (Modal call) 199. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.1.5 Argument specification 200. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2 CUSTOM MACRO BODY 202. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.1 Variables 202. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.2 Kind of Variables 203. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.3 Macro Instructions (G65) 208. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

15.2.4 Warning and Notes on Custom Macro 213. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.CUSTOM MACRO B 214. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.1 V ARIABLES 215. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.2 SYSTEM VARIABLES 218. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.3 ARITHMETIC AND LOGIC OPERATION 224. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–3

Table of Contents

B–62574EN/02

16.4 MACRO ST ATEMENTS AND NC STATEMENTS 228. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5 BRANCH AND REPETITION 229. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5.1 Unconditional Branch (GOTO Statement) 229. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5.2 Conditional Branch (IF Statement) 229. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.5.3 Repetition (While Statement) 230. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6 MACRO CALL 233. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.1 Simple Call (G65) 233. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.2 Modal Call (G66) 238. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.3 Macro Call Using G Code 240. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.4 Macro Call Using an M Code 241. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.5 Subprogram Call Using an M Code 242. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.6 Subprogram Calls Using a T Code 243. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.6.7 Sample Program 244. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.7 PROCESSING MACRO ST ATEMENTS 246. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.8 REGISTERING CUSTOM MACRO PROGRAMS 248. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.9 LIMITATIONS 249. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

16.10 EXTERNAL OUTPUT COMMANDS 250. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

17.PROGRAMMABLE PARAMETER ENTRY(G10) 254. . . . . . . . . . . . . . . . . . . . . . . . . . .

18.ROTARY AXIS ROLL–OVER 256. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

III OPERATION

1. GENERAL 259. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.1 MANUAL OPERATION 260. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.2 TOOL MOVEMENT BY PROGRAMING – AUTOMATIC OPERATION 262. . . . . . . . . . . . . . . . . . . .

1.3 AUTOMATIC OPERATION 263. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4 TESTING A PROGRAM 264. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4.1 Check by Running the Machine 264. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.4.2 How to View the Position Display Change without Running the Machine 265. . . . . . . . . . . . . . . . . . . . .

1.5 EDITING A PART PROGRAM 266. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.6 DISPLAYING AND SETTING DATA 267. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7 DISPLAY 270. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.1 Program Display (See III–11.2.1 and III–11.3.1) 270. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.2 Current Position Display (See III–11.1.1 to 11.1.3) 271. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.3 Alarm Display (See III–7.1) 271. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.7.4 Parts Count Display, Run Time Display (See III–11.1.5) 272. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.8 DATA OUTPUT (See III–8) 273. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2. OPERATIONAL DEVICES 274. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.1 CR T/MDI PANELS AND LCD/MDI PANELS 275. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.2 FUNCTION KEYS AND SOFT KEYS 278. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.2.1 General Screen Operations 278. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.2.2 Function Keys 279. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.2.3 Key Input and Input Buffer 280. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3 EXTERNAL I/O DEVICES 282. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.1 FANUC Handy File 284. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.2 FANUC Floppy Cassette 284. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–4

B–62574EN/02

2.3.3 FANUC FA Card 285. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.4 FANUC PPR 285. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.3.5 Portable Tape Reader 286. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4 POWER ON/OFF 287. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.1 Turning on the Power 287. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.2 Display of Software Configuration 288. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

2.4.3 Power Disconnection 288. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Table of Contents

3. MANUAL OPERATION 289. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.1 MANUAL REFERENCE POSITION RETURN 290. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.2 JOG FEED 292. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.3 INCREMENTAL FEED 294. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.4 MANUAL HANDLE FEED 295. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

3.5 MANUAL ABSOLUTE ON AND OFF 297. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4. AUTOMATIC OPERATION 302. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.1 MEMOR Y OPERATION 303. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.2 MDI OPERATION 305. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.3 DNC OPERATION 307. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.4 MIRROR IMAGE 308. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4.5 SEQUENCE NUMBER SEARCH 310. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5. TEST OPERATION 312. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.1 MACHINE LOCK AND AUXILIAR Y FUNCTION LOCK 313. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.2 FEEDRATE OVERRIDE 314. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.3 RAPID TRAVERSE OVERRIDE 315. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.4 DRY RUN 316. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

5.5 SINGLE BLOCK 317. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6. SAFETY FUNCTIONS 319. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.1 EMERGENCY STOP 320. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.2 OVERTRAVEL 321. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

6.3 STROKE CHECK 322. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7. ALARM AND SELF–DIAGNOSIS FUNCTIONS 324. . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.1 ALARM DISPLAY 325. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

7.2 CHECKING BY SELF–DIAGNOSTIC SCREEN 327. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8. DATA INPUT/OUTPUT 329. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.1 FILES 330. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.2 FILE SEARCH 332. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.3 FILE DELETION 333. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4 PROGRAM INPUT/OUTPUT 334. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.1 Inputting a Program 334. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.4.2 Outputting a Program 336. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5 OFFSET DAT A INPUT AND OUTPUT 339. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–5

Table of Contents

8.5.1 Inputting Offset Data 339. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.5.2 Outputting Offset Data 340. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–62574EN/02

8.6 INPUTTING AND OUTPUTTING PARAMETERS

AND PITCH ERROR COMPENSATION DATA 341. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.1 Inputting Parameters 341. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.6.2 Outputting Parameters 342. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.7 INPUTTING/OUTPUTTING CUSTOM MACRO B COMMON VARIABLES 343. . . . . . . . . . . . . . . .

8.7.1 Inputting Custom Macro B Common Variables 343. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

8.7.2 Outputting Custom Macro B Common Variable 344. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9. EDITING PROGRAMS 345. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1 INSERTING, ALTERING AND DELETING A WORD 346. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.1 Word Search 348. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.2 Heading a Program 350. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.3 Inserting a Word 351. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.4 Altering a Word 352. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.1.5 Deleting a Word 353. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2 DELETING BLOCKS 354. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.1 Deleting a Block 354. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.2.2 Deleting Multiple Blocks 355. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.3 PROGRAM NUMBER SEARCH 356. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4 DELETING PROGRAMS 357. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4.1 Deleting One Program 357. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.4.2 Deleting All Programs 357. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5 EXTENDED PART PROGRAM EDITING FUNCTION 358. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.1 Copying an Entire Program 359. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.2 Copying Part of a Program 360. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.3 Moving Part of a Program 361. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.4 Merging a Program 362. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.5 Supplementary Explanation for Copying, Moving and Merging 363. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.5.6 Replacement of Words and Addresses 364. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.6 BACKGROUND EDITING 366. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

9.7 REORGANIGING MEMORY 368. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.CREATING PROGRAMS 369. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.1 CREATING PROGRAMS USING THE MDI P ANEL 370. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

10.2 AUTOMATIC INSERTION OF SEQUENCE NUMBERS 371. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.SETTING AND DISPLAYING DATA 373. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–6

POS

PRGRM

(IN AUTO MODE OR MDI MODE) 389. . . . .

11.1 SCREENS DISPLAYED BY FUNCTION KEY

11.1.1 Position Display in the Work Coordinate System 381. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.2 Position Display in the Relative Coordinate System 382. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.3 Overall Position Display 384. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.4 Actual Feedrate Display 385. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.5 Display of Run Time and Parts Count 386. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.1.6 Operating Monitor Display 387. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2 SCREENS DISPLAYED BY FUNCTION KEY

11.2.1 Program Contents Display 389. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.2 Current Block Display Screen 390. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.3 Next Block Display Screen 391. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

381. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B–62574EN/02

Table of Contents

11.2.4 Program Check Screen 392. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.2.5 Program Screen for MDI Operation 393. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.3 SCREENS DISPLAYED BY FUNCTION KEY

11.3.1 Displaying Memory Used and a List of Programs 394. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4 SCREENS DISPLAYED BY FUNCTION KEY

11.4.1 Setting and Displaying the Tool Offset Value 397. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.2 Displaying and Setting the Workpiece Origin Offset Value 399. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.4.3 Displaying and Setting Custom Macro Common Variables 400. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5 SCREENS DISPLAYED BY FUNCTION KEY

11.5.1 Displaying and Setting Parameters 402. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5.2 Displaying and Setting Pitch Error Compensation Data 404. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5.3 Displaying and Entering Setting Data 409. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.5.4 Displaying and Setting Run Time,Parts Count 411. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.6 SCREENS DISPLAYED BY FUNCTION KEY

11.6.1 Displaying Operator Message 413. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.6.2 Displaying and Setting the Software Operator’s Panel 414. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

PRGRM

(IN THE EDIT MODE) 394. . . . . . . . . . . . . . . .

MENU OFSET

DGNOS PARAM

OPR

ALARM

11.7 DISPLA YING THE PROGRAM NUMBER, SEQUENCE NUMBER,

AND STATUS, AND W ARNING MESSAGES FOR DATA SETTING 416. . . . . . . . . . . . . . . . . . . . . .

11.7.1 Displaying the Program Number and Sequence Number 416. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

11.7.2 Displaying the Status and Warning for Data Setting 417. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

IV MAINTENANCE 419. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

397. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

401. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

413. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1. METHOD OF REPLACING BATTERY 421. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.1 REPLACING CNC BATTERY FOR MEMORY BACK–UP 422. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

1.2 REPLACING BATTERIES FOR ABSOLUTE PULSE CODER 423. . . . . . . . . . . . . . . . . . . . . . . . . . . .

APPENDIX

A. TAPE CODE LIST 427. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

B. LIST OF FUNCTIONS AND TAPE FORMAT 430. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

C. RANGE OF COMMAND VALUE 434. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D. NOMOGRAPHS 437. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D.1 TOOL PATH AT CORNER 438. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

D.2 RADIUS DIRECTION ERROR AT CIRCLE CUTTING 441. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

E. STATUS WHEN TURNING POWER ON, WHEN CLEAR AND WHEN RESET 442.

F. CHARACTER–TO–CODES CORRESPONDENCE TABLE 444. . . . . . . . . . . . . . . . . .

G. ALARM LIST 445. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

H. OPERATION OF PORTABLE TAPE READER 461. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

c–7

I. GENERAL

B–62574EN/02

0–D

GENERAL

This manual consists of the following parts:

1. GENERAL

  

I. GENERAL

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

II. PROGRAMMING

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

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 batteries.

APPENDIX

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

This manual does not describe parameters in detail. For details on parameters mentioned in this manual, refer to the manual for parameters (B–62580EN).

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 0–MD 0–MD FANUC Series 0–GSD 0–GSD

This manual uses the following symbols:





Indicates a combination of axes such as X__ Y__ Z (used in PROGRAMMING.).





Indicates the end of a block. It actually corresponds to the ISO code LF or EIA code CR.

–

1. GENERAL

GENERAL

B–62574EN/02

 

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

Table 1 Manuals Related to the FANUC Series 0–D

Manual name

FANUC Series 0–TD/MD/GCD/GSD CONNECTION MANUAL (HARDWARE)

FANUC Series 0–TD/MD/GCD/GSD CONNECTION MANUAL (FUNCTION)

FANUC Series 0–TD/GCD OPERATOR’S MANUAL B–62544EN FANUC Series 0–MD/GSD OPERATOR’S MANUAL B–62574EN

FANUC Series 0–TD/MD/GCD/GSD MAINTENANCE MANUAL

FANUC Series 0–TD/GCD PARAMETER MANUAL B–62550 FANUC Series 0–MD/GSD PARAMETER MANUAL B–62580EN

Specification

number

B–62543EN

B–62543EN–1

B–62545EN

B–62574EN/02

Cutting process

GENERAL

1. GENERAL

1.1

GENERAL FLOW OF OPERATION OF CNC MACHINE TOOL

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

1) First, prepare the program from a part drawing to operate the CNC machine tool. Store the program to a media appropriate for the CNC. 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.

Cuttin rocess

Cutting procedure

1. Cutting method : Rough Semi Finish

2. Cutting tools

3. Cutting conditions : Feedrate Cutting depth

4. Tool path

1 2 3

Feed cutting Side cutting

Hole machin-

ing

1. GENERAL

GENERAL

Tool

Side cutting

B–62574EN/02

Face cutting

Hole machining

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

B–62574EN/02

FANUC Series 0–MD

GENERAL

1. GENERAL

1.2

NOTES ON READING THIS MANUAL

NOTE

1 The function of an CNC machine tool system depends

not only on the CNC, but on the combination of the machine tool, its magnetic cabinet, the servo system, the CNC, the operator’s panels, etc. It is too difficult to describe the function, programming, and operation relating to all combinations. This manual generally describes these from the stand–point of the CNC. So, for details on a particular CNC machine tool, refer to the manual issued by the machine tool builder, which should take precedence over this manual.

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

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

3 Machining programs, parameters, variables, etc. are

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

4 This manual describes as many reasonable variations in

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

5 This manual describes the functions supported by the

software of the following versions and editions of FANUC Series 0–D. These functions may not be supported by other versions or editions of the software.

   

0471 04 or more

–

0472 01 or more

FANUC Series 0–GSD 0891 01 or more

6 This manual provides a general description of the

FANUC Series 0–D. Some functions described in this manual may not, therefore, be available depending on the software series or type.

II PROGRAMMING

B–62574EN/02

GENERAL

PROGRAMMING

1. GENERAL

PROGRAMMING

B–62574EN/02

1.1

TOOL MOVEMENT ALONG WORKPIECE PARTS FIGURE– INTERPOLATION

Explanations

D Tool movement along a

straight line

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

Tool

Workpiece

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

Program G01 X_ _ Y_ _ ; X_ _ ;

D Tool movement along an

arc

Program G03X_ _Y_ _R_ _;

Tool

Workpiece

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

B–62574EN/02

PROGRAMMING

1. GENERAL

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

(a) Movement along straight line

G01 Y__; X––Y––––;

Control unit

Interpolation

a) Movement

along straight line

b) Movement

along arc

Fig. 1.1 (c) Interpolation function

(b) Movement along arc

G03X––Y––R––;

X axis

Y axis

Tool movement

NOTE

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

1. GENERAL

PROGRAMMING

B–62574EN/02

1.2

FEED– FEED FUNCTION

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

mm/min

Workpiece

Table

Fig. 1.2 (a) Feed function

Tool

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

B–62574EN/02

1.3

PART DRAWING AND TOOL MOVEMENT

PROGRAMMING

1. GENERAL

1.3.1

Reference Position (Machine–Specific Position)



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

Reference position

Tool

Workpiece

Table

Fig. 1.3.1 (a) Reference position

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

Reference position return is performed by manual button operation.

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

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

1. GENERAL

1.3.2

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

PROGRAMMING

B–62574EN/02

Program

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

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

B–62574EN/02

PROGRAMMING

Coordinate system on part drawing established on the work-

Coordinate system specified by the CNC established on the table

Table

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

systemon part drawing

Workpiece

piece

1. GENERAL

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

1. GENERAL

PROGRAMMING

B–62574EN/02

D Methods of setting the

two coordinate systems in the same position

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

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

Fixed distance

Program zero point

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

Workpiece’s standard point

Fixed distance

(2) Mounting a workpiece directly against the jig

Program zero point

Jig

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

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

and pallet on the jig

Pallet

Jig

Workpiece

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

B–62574EN/02

1.3.3

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

PROGRAMMING

1. GENERAL

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

1. GENERAL

PROGRAMMING

B–62574EN/02

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–62574EN/02

PROGRAMMING

1. GENERAL

1.4

CUTTING SPEED – SPINDLE SPEED FUNCTION

Examples

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

Spindle speed

rpm

Workpiece

Tool

φD

V: Cutting speed

mm/min

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

S250;

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

1. GENERAL

PROGRAMMING

B–62574EN/02

1.5

SELECTION OF TOOL USED FOR VARIOUS MACHINING – TOOL FUNCTION

Examples

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

Tool number

01 02

A TC magazine

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

B–62574EN/02

PROGRAMMING

1. GENERAL

1.6

COMMAND FOR MACHINE OPERATIONS – MISCELLANEOUS FUNCTION

When machining is actually started, it is necessary to rotate the spindle, and feed coolant. For this purpose, on–off operations of spindle motor and coolant valve should be controlled (See II–11).

Tool

Coolant

Workpiece

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

1. GENERAL

PROGRAMMING

B–62574EN/02

1.7

PROGRAM CONFIGURATION

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

Block

Tool movement sequence

Block

Program

Block

⋅ ⋅ ⋅ ⋅

Block

Fig. 1.7 (a) Program configuration

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

B–62574EN/02

PROGRAMMING

1. GENERAL

Explanations

D Block

D Program

The block and the program have the following configurations.

1 block

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

Sequence number

Preparatory function

Dimension word Miscel-

laneous function

Fig. 1.7 (b) Block configuration

Spindle function

Tool function

End of block

A block has a sequence number at its head, which identifies the block, and an end–of–block code at the end, indicating the end of the block. This manual indicates the end–of–block code by ; (LF in the ISO code and CR in the EIA code).

;

ffff

⋅ ⋅ ⋅

M30 ;

Fig. 1.7 (c) Program configuration

Program number

Block Block Block

⋅ ⋅ ⋅

End of program

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

1. GENERAL

PROGRAMMING

B–62574EN/02

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

⋅

Hole #1

Hole #2

M99

Hole #2

B–62574EN/02

1.8

TOOL FIGURE AND TOOL MOTION BY PROGRAM

Explanations

PROGRAMMING

1. GENERAL

D Machining using the end

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

D Machining using the side

of cutter – Cutter compensation function (See II–14.2)

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

Standard tool

Workpiece

H3 H4

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

Cutter path using cutter compensation

Machined part figure

Workpiece

Cutter

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

1. GENERAL

PROGRAMMING

B–62574EN/02

1.9

TOOL MOVEMENT RANGE – STROKE

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

Table

Motor

Limit switch

Machine zero point

Specify these distances.

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

Besides strokes defined with limit switches, the operator can define an area which the tool cannot enter using a program or data in memory (see III–11). This function is called stroke check.

B–62574EN/02

 

PROGRAMMING

2. CONTROLLED AXES

2.1

PROGRAMMING

B–62574EN/02

CONTROLLED AXES

2.2

NAME OF AXES

2.3

INCREMENT SYSTEM

0–MD 0–GSD

No. of basic controlled axes Controlled axes expansion

(PMC axis is not included.) Basic simultaneously con-

trolled axes Simultaneously controlled

axes expansion

3 axes 3 axes

Max. 4 axes Max. 4 axis

4 axes 3 axes

Max. 4 axes Max. 3 axes

Names of the three basic axes are fixed as X, Y, and Z. Names of additional axes can be optionally selected from A, B, C, U, V, and W. They can be set by parameter No. 008 #2, #3, #4.

Name of incre-

ment system

IS–B 0.001mm

Least input increment Least command

0.0001inch

0.001deg

increment

0.001mm

0.0001inch

0.001deg

Maximum stroke

99999.999mm

9999.9999inch

99999.999deg

2.4

MAXIMUM STROKE

Name of incre-

ment system

IS–C 0.0001mm

Least input increment Least command

0.00001inch

0.00001deg

increment

0.0001mm

0.00001inch

0.00001deg

Maximum stroke

9999.9999mm

999.99999inch

9999.9999deg

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

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

B–62574EN/02

3. PREP ARATORY FUNCTION

PROGRAMMING

   

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

Type Meaning

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

specified.

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

same group is specified.

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

(G FUNCTION)

Explanations

G01X 

Z  X 

G00Z 

1. Modal G codes have the following initial conditions when the power is turned on or the system is reset to the clear state (bit 6 of parameter No. 045).

1) Those G codes marked

2) G20 and G21 retain their original conditions.

3) G00 or G01 is automatically selected depending on the setting of

bit 6 of parameter No. 011.

4) G90 or G91 is automatically selected depending on the setting of

bit 7 of parameter No. 030.

2. The G codes of group 00, except G10 and G11, are one–shot G codes.

3. If a G code that does not appear in the G code list is specified, or a G code whose options are not supported is specified, alarm No. 010 is displayed.

4. Multiple G codes of different groups can be specified in a single block. When multiple G codes of one group are specified in a block, the G code specified last is effective.

5. If any G code of group 01 is specified in a canned cycle mode, the canned cycle is automatically cancelled and the G80 condition is entered. However, a G code of group 01 is not affected by any of the

canned cycle G codes.

6. A G code is displayed from each group.

G01 is effective in this range.

in T able 3 are specified automatically .

3. PREP ARATORY FUNCTION

(G FUNCTION)

G code

G00

G01 G02 G03 Circular interpolation CCW G04 G09 G10 G11 Data setting mode cancel

G17 G18 G19 G20 G21 G27 G28 G29 00 Return from reference position G30 2nd reference position return G31 Skip function (0–GSD) G40 G41 G42 Cutter compensation right G43 G44 G49 G52 G53 G54 G55 G56 G57 G58 Workpiece coordinate system 5 selection G59 Workpiece coordinate system 6 selection G60 00 Single direction positioning G61 G62 G63 G64 G65 00 Macro call

PROGRAMMING

T able 3 G code list (1/2)

Group Function

Positioning Linear interpolation Circular interpolation CW

Dwell, Exact stop Exact stop Data setting

XpY p plane selection Xp: X axis or its parallel axis ZpXp plane selection Yp: Y axis or its parallel axis

02 Y pZp plane selection Zp: Z axis or its parallel axis

Input in inch Input in mm Reference position return check Return to reference position

Cutter compensation cancel

Cutter compensation left

Tool length compensation + direction Tool length compensation – direction Tool length compensation cancel Local coordinate system setting Machine coordinate system selection Workpiece coordinate system 1 selection Workpiece coordinate system 2 selection Workpiece coordinate system 3 selection Workpiece coordinate system 4 selection

Exact stop mode Automatic corner override Tapping mode Cutting mode

B–62574EN/02

3. PREP ARATORY FUNCTION

PROGRAMMING

T able 3 G code list (2/2)

G code

G66

G67 G73 G74 G75 01 Plunge grinding cycle (0–GSD)

G76 G77 G78 01 Continuous–feed surface grinding cycle (0–GSD) G79 Intermittent–feed surface grinding cycle (0–GSD)

G80 G81

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

G92 00 G94

G98 G99 G150

G151 G152 Normal direction control right side on (0–GSD)

G160 G161

Group Function

Macro modal call Macro modal call cancel Peck drilling cycle Counter tapping cycle

05 Feed per minute 1

Fine boring cycle Direct constant–dimension plunge grinding cycle (0–GSD)

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

Tapping cycle

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

speed

Return to initial point in canned cycle Return to R point in canned cycle Normal direction control cancel mode (0–GSD) Normal direction control left side on (0–GSD)

In–feed control function cancel (0–GSD) In–feed control function (0–GSD)

(G FUNCTION)

4. INTERPOLA TION FUNCTIONS

 

PROGRAMMING

B–62574EN/02

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.1

Positioning (G00)

Format

Explanations

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

G00 _;

IP IP

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

position, and for an incremental command, the dis– tance the tool moves.

Tool path generally does not become a straight line.

Start position

Restrictions

End position

Non liner positioning.

The rapid traverse rate in the G00 command is set to the parameter No. 518 to 521 for each axis independently by the machine tool builder. In the positioning mode actuated by G00, the tool is accelerated to a predetermined speed at the start of a block and is decelerated at the end of a block. Execution proceeds to the next block after confirming the in–position. ”In–position” means that the feed motor is within the specified range. This range is determined by the machine tool builder by setting to parameter No. 500 to 503.

The rapid traverse rate cannot be specified in the address F.

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62574EN/02

4.2

SINGLE DIRECTION POSITIONING (G60)

Format

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

Overrun

Start position

End position

G60 _;

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

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

Temporary stop

Explanations

Restrictions

An overrun and a positioning direction are set by the parameter (No. 029 #0 to #3, No. 204 to 207). Even when a commanded positioning direction coincides with that set by the parameter, the tool stops once before the end point.



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

in Z axis.

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

overrun has been set by the parameter.

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

positioning is not performed.

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

the canned cycles of G76 and G87.

B–62574EN/02

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.3

LINEAR INTERPOLATION (G01)

Format

Explanations

Tools can move along a line

G01 _F_;IP

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

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

F_:Speed of tool feed (Feedrate)

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

G01 α α β β γ γ ζ ζ

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 + 

) 2) 2) 

Ff ;



F +



F+



F +



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 αandβ 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 formula, then the β –axis feedrate unit is changed to deg 1min.

4. INTERPOLA TION FUNCTIONS

PROGRAMMING

B–62574EN/02

A calculation 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 (min)

268.3

degńmin

0.14907

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

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

Y axis

100.0

(End position)

D   

 

(Start position)

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

(End point)

200.00

(Start point)

90,

Feedrate is 300 deg/min

X axis

B–62574EN/02

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.4

CIRCULAR INTERPOLATION (G02,G03)

Format

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

Arc in the XpYp plane

G17

Arc in the ZpXp plane

G18

Arc in the YpZp plane

G19

G02 G03

Xp_Yp_

Xp_Zp_

Yp_Zp_

I_J_ R_

I_K_ R_

J_K_

F_;

F_ ;

Table.4.4 Description of the Command Format

Command

Description

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

Command values of X axis or its parallel axis Command values of Y axis or its parallel axis Command values of Z axis or its parallel axis

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

sign

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

4. INTERPOLA TION FUNCTIONS

Explanations

PROGRAMMING

B–62574EN/02

D    



D    



D    

     

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

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

pXp

in the positive–to–negative direction of the Z

axis (Yp axis or Xp axis,

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

G03

G02

G17

Xp Zp

G03

G02

G18

G03

G02

G19

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

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

End point (x,y)

Center

Start point

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

End point (z,x)

Center

Start

point

End point (y ,z)

Center

are omitted (the end

Start point

point is the same as the start point) and the center is specified with I, J, and K, a 360° arc (circle) is specified. 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.876), an alarm (No.020) occurs. (Valid only when bit 6 of parameter No. 393 is set to 1.)

B–62574EN/02

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

D  

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

For arc (1) (less than 180_)

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

For arc (2) (greater than 180°)

G91 G02 X

60.0 YP20.0 R–50.0 F300.0 ;

)

r=50mm

End point

(1)

D 

Restrictions

Start point

r=50mm

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

If I, J, K, and R addresses are specified simultaneously, the arc specified by address R takes precedence and the other are ignored. If an axis not comprising the specified plane is commanded, an alarm is displayed. For example, if axis U is specified as a parallel axis to X axis when plane XY is specified, an alarm (No.028)is displayed. When an arc having a center angle close to 180ø is specified using its radius R, the system may fail to calculate the center of the arc correctly. Therefore, specify the arc with I, J, and K.

4. INTERPOLA TION FUNCTIONS

Examples

PROGRAMMING

Y axis

100

B–62574EN/02

50R

60 40

90 120 140 200

60R

The above tool path can be programmed as follows ;

(1) In absolute programming

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



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

(2) In incremental programming

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



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

X axis

B–62574EN/02

PROGRAMMING

4. INTERPOLA TION FUNCTIONS

4.5

SKIP FUNCTION (G31) (FOR 0–GSD ONLY)

Format

Explanations

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

G31 _ ;

G31

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

which it is specified)

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

#5061 X axis coordinate value #5062 Y axis coordinate value #5063 Z axis coordinate value

WARNING

Disable feedrate override, dry run, and automatic acceleration/deceleration (These operations can be validated by setting bit 3 of parameter No. 015 to 1.) when the feedrate per minute is specified, allowing for an error in the position of the tool when a skip signal is input. These functions are enabled when the feedrate per rotation is specified.

NOTE

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

4. INTERPOLA TION FUNCTIONS

Examples D The next block to G31 is

an incremental command

PROGRAMMING

G31 G91X100.0 F100;

Y50.0;

B–62574EN/02

Y50.0

D The next block to G31 is

an absolute command for 1 axis

Skip signal is input here

Fig.4.5 (a) The next block is an incremental command

G31 G90X200.00 F100;

Y100.0;

Skip signal is input here

100.0

50.0

Actual motion Motion without skip signal

Y100.0

X200.0

D The next block to G31 is

an absolute command for 2 axes

Actual motion

Motion without skip signal

Fig.4.5 (b) The next block is an absolute command for 1 axis

G31 G90X200.0 F100;

X300.0 Y100.0;

Skip signal is input here

100

100 200 300

Fig 4.5 (c) The next block is an absolute command for 2 axes

(300,100)

Actual motion

Motion without skip signal

B–62574EN/02

 

PROGRAMMING

5. FEED FUNCTIONS

PROGRAMMING

B–62574EN/02

5.1

GENERAL

D Feed functions

D Override

D Automatic acceleration/

deceleration

Rapid traverse rate :

Feed rate

RMAX

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. 518 to 521).

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)).

Linear acceleration/deceleration (constant acceleration)

RMAX

: Rapid traverse rate

: Acceleration/deceleration

time constant for rapid traverse rate

Jog feed :

Exponential acceleration/deceleration (constant time constant)

Cutting feed, dry run :

Time

FJ : Jog feed rate

Acceleration/deceleration time constant

J :

FL : Deceleration stop feed for jog feed rate

Time

Exponential acceleration/deceleration (constant time constant)

Cuting feedrate, dry run rate

C :

Acceleration/deceleration time constant for feedrate

C :

Time

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

B–62574EN/02

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)).

∆ r: Error

Programmed path Actual tool path

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

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

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

the tool to move as programmed.

5. FEED FUNCTIONS

5.2

RAPID TRAVERSE

Format

PROGRAMMING

G00 _ ;

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

_ ; Dimension word for the end point

B–62574EN/02

Explanations

D Command value range of

rapid traverse rate

The positioning command (G00) positions the tool by rapid traverse. In rapid traverse, the next block is executed after the specified feedrate becomes 0 and the servo motor reaches a certain range set by the machine tool builder (in–position check). (In–position check can be disabled for each block by setting bit 5 of parameter No. 020 to 1.) A rapid traverse rate is set for each axis by parameter No. 518 to 521, so no rapid traverse feedrate need be programmed. The following overrides can be applied to a rapid traverse rate with the switch on the machine operator’s panel:F0, 25, 50, 100% F0: Allows a fixed feedrate to be set for each axis by parameter No. 533. For detailed information, refer to the appropriate manual of the machine tool builder.

Increment system

IS–B IS–C

Metric output

Inch output

30 to 100,000 mm/min 30 to 100,000 deg/min

3.0 to 4,000.0 inch/min

3.0 to 100,000 deg/min

30 to 24,000 mm/min 30 to 24,000 deg/min

3.0 to 960.0 inch/min

3.0 to 24,000 deg/min

B–62574EN/02

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

G94 ; G code (group 05) for 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

Starting point

D Feed per minute (G94)

Start point

Linear interpolation

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

Center

Circular interpolation

End point

After specifying G94 (in the feed per minute mode), the amount of feed of the tool per minute is to be directly specified by setting a number after F. G94 is a modal code. At power–on, the feed per minute mode is set. An override from 0% to 150% (in 10% steps) can be applied to feed per minute with the switch on the machine operator’s panel. For detailed information, see the appropriate manual of the machine tool builder.

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

Tool

Workpiece

Table

Fig. 5.3 (b) Feed per minute

WARNING

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

5. FEED FUNCTIONS

PROGRAMMING

< Command value range of feed per minute >

Increment system

IS–B IS–C

B–62574EN/02

D Cutting feedrate clamp

Metric input

Inch input

1 to 100,000 mm/min 1 to 100,000 deg/min

0.01 to 4,000.0 inch/min

0.01 to 6,000.0 deg/min

1 to 12,000 mm/min 1 to 12,000 deg/min

0.01 to 480.0 inch/min

0.01 to 600.0 deg/min

When a value with a decimal fraction is specified in a feedrate command for feed per minute, the value is valid within the following range. To specify a value that falls outside this range, specify an integer.

Increment system

IS–B IS–C

Metric input

Inch input

0.001 to 99,999.999 mm/min

0.001 to 99,999.999 deg/min

0.00001 to 999.99999 inch/min

0.00001 to 999.99999 deg/min

0.001 to 12,000.000 mm/min

0.001 to 12,000.000 deg/min

0.00001 to 480.00000 inch/min

0.00001 to 600.00000 deg/min

A common upper limit can be set on the cutting feedrate along each axis with parameter No. 527. If an actual cutting feedrate (with an override applied) exceeds a specified upper limit, it is clamped to the upper limit.

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–62574EN/02

PROGRAMMING

5. FEED FUNCTIONS

5.4

CUTTING FEEDRATE CONTROL

Function name

Exact stop

Cutting mode

Tapping mode

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

Table 5.4(a) Cutting Feedrate Control

G code Validity of G code Description

G09

G61

G64

G63

This function is valid for specified blocks only.

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

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

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

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

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

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

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). In–position check can be disabled by setting bit 5 of parameter No. 020 to 1.

2. Inner corner angle θ: 2°

< θ x α x 178°

(α is a set value)

Workpiece

Tool

Exact stop G09 IP_ ;

Cutting mode G64 ;

G61 ;

Tapping mode G63 ;

5. FEED FUNCTIONS

5.4.1

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

PROGRAMMING

B–62574EN/02

Explanations

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

(2)

(1)

Fig. 5.4.1 (a) 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 or tapping mode

CAUTION

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

B–62574EN/02

PROGRAMMING

5. FEED FUNCTIONS

5.4.2

Internal Circular Cutting Feedrate Change

For internally offset circular cutting, the feedrate on a programmed path is set to a specified feedrate (F) by specifying the circular cutting feedrate with respect to F , as indicated below (Fig. 5.4.2(a)). 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(a) Internal circular cutting feedrate change

path

If Rc is much smaller than Rp, Rc/Rp80; the tool stops. A minimum deceleration ratio (MDR) is to be specified with parameter No. 213. When Rc/Rp

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

CAUTION

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

×(feedrate override)

(automatic override for the inner corners)

5. FEED FUNCTIONS

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)

B–62574EN/02

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

IS–B

IS–C

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

Increment system

IS–B 1 to 99999999 0.001 s IS–C 1 to 99999999 0.0001 s

Command value range Dwell time unit

0.001 to 99999.999 s

0.0001 to 9999.9999

Command value range Dwell time unit

B–62574EN/02

General

PROGRAMMING

 

6. REFERENCE POSITION

D Reference position

The reference position is a fixed position on a machine tool to which the tool can easily be moved by the reference position return function. For example, the reference position is used as a position at which tools are automatically changed. Up to two reference positions can be specified by setting coordinates in the machine coordinate system in parameters. The first reference position must be the machine zero point.

2nd reference position

Machine zero point (1st reference position)

Fig. 6 (a) Machine zero point and reference positions

6. REFERENCE POSITION

PROGRAMMING

B–62574EN/02

D Reference position

return and movement from the reference position

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

Reference position return A→B→R Return from the reference position R→B→C

B (Intermediate position)

A (Start position for reference position return)

Fig. 6 (b) Reference position return and return form the reference position

C (Destination of return from the reference position)

R (Reference position)

D Reference position

return check



D Reference position

return

D Return from reference

position

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

 _

    _

: Command specifying the intermediate position

(Absolute/incremental command)

   _

Reference position return

2nd reference position return

(P2 can be omitted.)

: Command specifying the destination of return from reference

position (Absolute/incremental command)

D Reference position

return check

7 _

: Command specifying the reference position

(Absolute/incremental command)

B–62574EN/02



PROGRAMMING

6. REFERENCE POSITION

D Reference position

return (G28)

D 2nd reference position

return (G30)

D Return from the

reference position (G29)

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

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

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

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

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

D Reference position

return check (G27)

Restrictions D Status the machine lock

being turned on

D First return to the

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

G27 command positions the tool at rapid traverse rate. If the tool reaches the reference position, the reference position return lamp lights up. However, if the position reached by the tool is not the reference position, an alarm (No. 092) is displayed.

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

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 ( No. 003 #0 to #3). Therefore the specified intermediate position must be a position to which reference position return is possible.

6. REFERENCE POSITION

PROGRAMMING

B–62574EN/02

D Reference position

return check in an offset mode

D Lighting the lamp when

the programmed position does not coincide with the reference position



D Manual reference

position return

Examples

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

When the machine tool system is an inch system with metric input, the reference position return lamp may also light up even if the programmed position is shifted from the reference position by 1µ. This occurs because the least input increment of the machine tool system is smaller than its least command increment.

See III–3.1.

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

The tool is changed at the reference position

Reference position

500

300 200

Fig. 6 (c) Reference position return and return from the reference position

200 1000 1300

B–62574EN/02

PROGRAMMING

 

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

X_Y_Z_

This command is referred to as a dimension word.

7. COORDINA TE SYSTEM

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_.

7. COORDINA TE SYSTEM

PROGRAMMING

B–62574EN/02

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. The machine zero point matches the first reference position. 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, but the incremental command G91 is ignored. When the tool is to be moved to a machine–specific position such as a tool change position, program the movement in a machine coordinate system based on G53.

Restrictions

D Cancel of the

compensation function

D G53 specification

immediately after power–on

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

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

B–62574EN/02

PROGRAMMING

7. COORDINA TE SYSTEM

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. 010 #7 is set beforehand, a workpiece coordinate system is automatically set when manual reference position return is performed (see III–3.1.).

(3) Input using the CRT/MDI panel

Six workpiece coordinate systems can be set beforehand using the CRT/MDI panel (see III–11.4.3.).

To use absolute programming, establish a workpiece coordinate system by applying one of the methods described above.

Format

Setting a workpiece coordinate system by G92

Explanations

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

Examples

Example 1

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

23.0

25.2

G92 _IP

Example 2

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

1200.0

Base point

If an absolute command is isĆ sued, the base point moves to the commanded position.  In order to move the tool tip to the commanded position, the  difĆ ference from the tool tip to the base point is compensated by tool length offset.

600.0

7. COORDINA TE SYSTEM

PROGRAMMING

B–62574EN/02

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 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

CRT/MDI panel

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

G54 Workpiece coordinate system 1. . . .

G55 Workpiece coordinate system 2. . . .

G56 Workpiece coordinate system 3. . . .

G57 Workpiece coordinate system 4. . . .

G58 Workpiece coordinate system 5. . . .

G59 Workpiece coordinate system 6. . . .

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

G90 G55 G00 X40.0 Y100.0 ;

Workpiece coordinate system 2 (G55)

100.0

40.0

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

Fig. 7.2.2 (a)

B–62574EN/02

PROGRAMMING

7. COORDINA TE SYSTEM

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. Four methods are available to change an external workpiece zero point offset value or workpiece zero point offset value. (1) Inputting from the CRT/MDI panel (see III–11.4.2) (2) Programming by G10 or G92 (3) Changing an external workpiece zero point offset value (refer to

machine tool builder’s manual)

(4) System variables by Custom Macro B

Workpiece coordinate system 1 (G54)

ZOFS1

Machine zero

Workpiece coordinate system 2 (G55)

ZOFS2

EXOFS

Workpiece coordinate system 3 (G56)

ZOFS3

ZOFS4 ZOFS5

ZOFS6

Workpiece coordinate system 4 (G57)

Workpiece coordinate system 5 (G58)

Workpiece coordinate system 6 (G59)

Format

Changing by G10

Changing by G92

Explanations

D Changing by G10

EXOFS : External workpiece zero point offset value ZOFS1 to ZOFS6 : Workpiece zero point offset value

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

workpiece zero point offset value

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

: Workpiece zero point offset value of each axis

G92 _;IP

With the G10 command, each workpiece coordinate system can be changed separately. When an absolute workpiece zero point offset value is specified, the specified value becomes a new offset value. When an incremental workpiece zero point offset value is specified, the specified value is added to the current offset value to produce a new offset value.

7. COORDINA TE SYSTEM

PROGRAMMING

B–62574EN/02

D Changing by G92



160

100

By specifying G92IP_;, a workpiece coordinate system (selected with a code from G54 to G59) is shifted to set a new workpiece coordinate system so that the current tool position matches the specified coordinates ( IP_). Then, the amount of coordinate system shift is added to all the workpiece zero point offset values. This means that all the workpiece coordinate systems are shifted by the same amount.

WARNING

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

YȀY

G54 workpiece coordinate system

Tool position

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

G54 Workpiece coordinate system

1200.0

X’ – Z’ New workpiece coordinate system X – Z Original workpiece coordinate system A : Offset value created by G92 B : G54 workpiece zero point offset value C : G55 workpiece zero point offset value

100

Z’

600.0

100

200

1200.0

New workpiece coordinate system

XȀ

Original workpiece coordinate system

G55 Workpiece coordinate system

ZȀ

600.0

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

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

B–62574EN/02

PROGRAMMING

7. COORDINA TE SYSTEM

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. To 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.

(Local coordinate system)

IP_

(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)

IP_

(G59 : Workpiece coordinate system 6)

7. COORDINA TE SYSTEM

PROGRAMMING

B–62574EN/02

WARNING

1 When an axis returns to the reference point by the

manual reference point return function, the zero point of the local coordinate system of the axis matches that of the work coordi–nate system. The same is true when the following command is issued:

G52α0;

α:Axis which returns to the reference point

2 The local coordinate system setting does not change the

workpiece and machine coordi–nate systems.

3 The local coordinate system is cancelled when the reset

operation is performed.

4 When setting a workpiece coordinate system with the

G92 command, the local coordinate systems are cancelled.

5 G52 cancels the offset temporarily in cutter

compensation.

6 Command a move command immediately after the G52

block in the absolute mode.

B–62574EN/02

PROGRAMMING

7. COORDINA TE SYSTEM

7.4

PLANE SELECTION

Explanations

Select the planes for circular interpolation, cutter compensation, and drilling by G–code. The following table lists G–codes and the planes selected by them.

T able 7.4 Plane selected by G code

G code

G17 Xp Yp plane G18 Zp Xp plane axis parallel G19 Yp Zp plane

Selected

plane

Xp Yp Zp

X–axis or an Y–axis or an Z–axis or an

axis parallel

to it to it to it

axis parallel

Xp, Yp, Zp are determined by the axis address appeared in the block in which G17, G18 or G19 is commanded. When an axis address is omitted in G17, G18 or G19 block, it is assumed that the addresses of basic three axes are omitted. Parameter No. 279 is used to specify that an optional axis be parallel to the each axis of the X, Y–, and Z–axes as the basic three axes. The plane is unchanged in the block in which G17, G18 or G19 is not commanded.

Examples

Plane selection when the X–axis is parallel with the U–axis.

G17X_Y_ XY plane, G17U_Y_ UY plane G18X_Z_ ZX plane X_Y_ Plane is unchanged (ZX plane) G17 XY plane G18 ZX plane G17 U_ UY plane G18Y_ ; ZX plane, Y axis moves regardless without any

relation to the plane.

NOTE

When the system is turned on or placed in the clear state by a reset (bit 6 of parameter No. 045), G17, G18, or G19 is selected according to the setting of parameter No. 212.

8. COORDINA TE VALUE AND DIMENSION

   

This chapter contains the following topics.

8.1 ABSOLUTE AND INCREMENT AL PROGRAMMING (G90, G91)

8.2 INCH/METRIC CONVERSION (G20, G21)

8.3 DECIMAL POINT PROGRAMMING

PROGRAMMING

B–62574EN/02

PROGRAMMING

8. COORDINA TE VALUE AND DIMENSION

8.1

ABSOLUTE AND INCREMENTAL PROGRAMMING (G90, G91)





There are two ways to command travels of the tool; the absolute command, and the incremental command. In the absolute command, coordinate value of the end position is programmed; in the incremental command, move distance of the position itself is programmed. G90 and G91 are used to command absolute or incremental command, respectively.

Absolute command Incremental command

G90 X40.0 Y70.0 ; G91 X–60.0 Y40.0 ;

70.0

G90 _ ; G91 _ ;IPIP

Absolute command Incremental command

End position

30.0

40.0 100.0

Start position

8. COORDINA TE VALUE AND DIMENSION

PROGRAMMING

B–62574EN/02

8.2

INCH/METRIC CONVERSION(G20,G21)



Either inch or metric input can be selected by G code.

G20 ; G21 ;

Inch input mm input

This G code must be specified in an independent block before setting the coordinate system at the beginning of the program.

After the G code for inch/metric conversion is specified, the unit of input data is switched to the least inch or metric input increment of increment system IS–B or IS–C (2.3). The unit of data input for degrees remains unchanged.The unit systems for the following values are changed after inch/metric conversion:

– Feedrate commanded by F code – Positional command – Work zero point offset value – Tool compensation value – Unit of scale for manual pulse generator – Movement distance in incremental feed – Some parameters

When the power is turned on, the G code is the same as that held before the power was turned off.

WARNING

1 G20 and G21 must not be switched during a program. 2 When switching inch input (G20) to metric input (G21)

and vice versa, the tool compensation value must be re–set according to the least input increment.

CAUTION

Reference position return is performed at a low speed for the first G28 command after the inch input is switched to the metric input or vice versa.

NOTE

1 When the least input increment and the least command

increment systems are different, the maximum error is half of the least command increment. This error is not accumulated.

2 The inch and metric input can also be switched using

settings.

B–62574EN/02

PROGRAMMING

8. COORDINA TE VALUE AND DIMENSION

8.3

DECIMAL POINT PROGRAMMING





Numerical values can be entered with a decimal point. A decimal point can be used when entering a distance, time, or speed. Decimal points can be specified with the following addresses: X, Y, Z, U, V, W, A, B, C, I, J, K, Q, R, and F.

There are two types of decimal point notation: calculator–type notation and standard notation. When calculator–type decimal notation is used, a value without decimal point is considered to be specified in mm, inch, or deg. When standard decimal notation is used, such a value is considered to be specified in least input increments.Select either calculator–type or standard decimal notation by using the parameter No. 051#7. Values can be specified both with and without decimal point in a single program.

Program command Pocket calculator

X1000 Command value without decimal point

type decimal point

programming

1000mm Unit : mm

Standard type decimal

point programming

1mm Unit : Least input increment

(0.001 mm)

X1000.0 Command value with decimal point

WARNING

In a single block, specify a G code before entering a value. The position of decimal point may depend on the command.

Examples: G20; Input in inches X1.0 G04; X1.0 is considered to be a distance and

G04 X1.0; Equivalent to G04 X1000. The tool dwells

1000mm Unit : mm

processed as X10000. This command is equivalent to G04 X10000. The tool dwells for 10 seconds.

for one second.

8. COORDINA TE VALUE AND DIMENSION

NOTE

PROGRAMMING

B–62574EN/02

1 Fractions less than the least input increment are

truncated.

Examples: X1.2345; Truncated to X1.234 when the least input

increment is 0.001 mm. Processed as X1.2345 when the least input increment is 0.0001 inch.

2 When more than eight digits are specified, an alarm

occurs. If a value is entered with a decimal point, the number of digits is also checked after the value is converted to an integer according to the least input increment.

Examples: X1.23456789; Alarm 003 occurs because more than eight

digits are specified.

X123456.7; If the least input increment is 0.001 mm, the

value is converted to integer 123456700. Because the integer has more than eight digits, an alarm occurs.

B–62574EN/02

9. SPINDLE SPEED FUNCTION

PROGRAMMING

SPINDLE SPEED FUNCTION (S FUNCTION)

The spindle speed can be controlled by specifying a value following address S. This chapter contains the following topics.

9.1 SPECIFYING THE SPINDLE SPEED WITH A CODE

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

(S FUNCTION)

9. SPINDLE SPEED FUNCTION (S FUNCTION)

PROGRAMMING

B–62574EN/02

9.1

SPECIFYING THE SPINDLE SPEED WITH A BINARY CODE

9.2

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

A 2–digit S code can be specified in a block. For a description of the use of S codes, such as their execution sequence in a block in which a spindle speed, move command, and S code are specified, see the manual provided by the machine tool builder.

The spindle speed can be specified directly by address S followed by a five–digit value (rpm). The unit for specifying the spindle speed may vary depending on the machine tool builder. Refer to the appropriate manual provided by the machine tool builder for details.

B–62574EN/02

PROGRAMMING

   

Tool Selection function is available at tool function.

10. TOOL FUNCTION (T FUNCTION)

PROGRAMMING

B–62574EN/02

10.1

TOOL SELECTION FUNCTION

By specifying two or four–digit numerical value following address T, tools can be selected on the machine. One T code can be commanded in a block. Refer to the machine tool builder’s manual for the number of digits commandable with address T and the correspondence between the T codes and machine operations. When a move command and a T code are specified in the same block, the commands are executed in one of the following two ways: (i) Simultaneous execution of the move command and T function

commands.

(ii) Executing T function commands upon completion of move

command execution. The selection of either (i) or (ii) depends on the machine tool builder’s specifications. Refer to the manual issued by the machine tool builder for details.

B–62574EN/02

PROGRAMMING

 

There are two types of auxiliary functions ; miscellaneous function (M code) for specifying spindle start, spindle stop program end, and so on, and secondary auxiliary function (B code ) for specifying index table positioning. When a move command and miscellaneous function are specified in the same block, the commands are executed in one of the following two ways: i) Simultaneous execution of the move command and miscellaneous

function commands.

ii) Executing miscellaneous function commands upon completion of

move command execution. The selection of either sequence depends on the machine tool builder’s specification. Refer to the manual issued by the machine tool builder for details.

1 1. AUXILIAR Y FUNCTION

PROGRAMMING

B–62574EN/02

11.1

AUXILIARY FUNCTION (M FUNCTION)

Explanations

D M02,M03

(End of program)

When a three–digid numeral is specified following address M, code signal and a strobe signal are sent to the machine. The machine uses these signals to turn on or off its functions. Usually, only one M code can be specified in one block. In some cases, however, up to three M codes can be specified for some types of machine tools. Which M code corresponds to which machine function is determined by the machine tool builder. All M codes are processed in the machine except for M98, M99, M codes for calling a subprogram, and M codes for calling a custom macro. Refer to the machine tool builder’s instruction manual for details.

The following M codes have special meanings.

This indicates the end of the main program Automatic operation is stopped and the CNC unit is reset. This differs with the machine tool builder. After a block specifying the end of the program is executed, control returns to the start of the program. Bit 5 of parameter 019 (M02) can be used to disable M02 from returning control to the start of the program.

D M00

(Program stop)

D M01

(Optional stop)

D M98

(Calling of sub-

program)

D M99

(End of subprogram)

Automatic operation is stopped after a block containing M00 is executed. When the program is stopped, all existing modal information remains unchanged. The automatic operation can be restarted by actuating the cycle operation. This differs with the machine tool builder.

Similarly to M00, automatic operation is stopped after a block containing M01 is executed. This code is only effective when the Optional Stop switch on the machine operator’s panel has been pressed.

This code is used to call a subprogram. The code and strobe signals are not sent. See the subprogram

This code indicates the end of a subprogram. M99 execution returns control to the main program. See the subprogram

section 12.3 for details.

NOTE

The block following M00, M01, M02 and M30, is not read into the input buffer register, if present. Similarly, two M codes which do not buffer can be set by parameters (Nos. 111 to 112). Refer to the machine tool builder’s instruction manual for these M codes.

section 12.3 for details .

B–62574EN/02

PROGRAMMING

1 1. AUXILIAR Y FUNCTION

11.2

MULTIPLE M COMMANDS IN A SINGLE BLOCK

Explanations

So far, one block has been able to contain only one M code. However , this function allows up to three M codes to be contained in one block. Up to three M codes specified in a block are simultaneously output to the machine. This means that compared with the conventional method of a single M command in a single block, a shorter cycle time can be realized in machining. To use this function, set bit 7 of parameter No. 065 to 1.

CNC allows up to three M codes to be specified in one block. However, some M codes cannot be specified at the same time due to mechanical operation restrictions. M00, M01, M02, M30, M98 or M99 must not be specified together with another M code. Some M codes other than M00, M01, M02, M30, M98, and M99 cannot be specified together with other M codes; each of those M codes must be specified in a single block. Such M codes include these which direct the CNC to perform internal operations in addition to sending the M codes themselves to the machine. T o be specified, such M codes are M codes for calling program numbers 9001 to 9009 and M codes for disabling advance reading (buffering) of subsequent blocks. Meanwhile, multiple of M codes that direct the CNC only to send the M codes themselves (without performing internal operations ) can be specified in a single block.

Examples

One M command

in a single block

M40 ; M50 ; M60 ;

G28G91X0Y0Z0 ;

: : :

Multiple M commands

in a single block

M40M50M60 ;

G28G91X0Y0Z0 ;

: : : : :

1 1. AUXILIAR Y FUNCTION

1 1.3

THE SECOND AUXILIARY FUNCTIONS (B CODES) (FOR 0–MD ONLY)

PROGRAMMING

Indexing of the table is performed by address B and a following 3 or 6–digit number. The relationship between B codes and the corresponding indexing differs between machine tool builders. Refer to the manual issued by the machine tool builder for details.

B–62574EN/02

Restrictions

When this functions is used, the B address specifying an axis movement disabled.

B–62574EN/02

General

PROGRAMMING

 

12. PROGRAM CONFIGURA TION

D Main program and

subprogram

There are two program types, main program and subprogram. Normally , the CNC operates according to the main program. However, when a command calling a subprogram is encountered in the main program, control is passed to the subprogram. When a command specifying a return to the main program is encountered in a subprogram, control is returned to the main program.

Main program

Instruction 1 Instruction 2

Follow the direction of the subprogram

Instruction n Instruction n+1

Subprogram

Instruction 1Ȁ

Instruction 2Ȁ

Return to the main program

Fig. 12 (a) Main program and Subprogram

The CNC memory can hold up to 200 main programs and subprograms (63 as standard). A main program can be selected from the stored main programs to operate the machine. See Chapter 10 in OPERA TION for the methods of registering and selecting programs.

12. PROGRAM CONFIGURA TION

PROGRAMMING

B–62574EN/02

D Program components

A program consists of the following components:

T able 12 (a) Program components

Components

Tape start Symbol indicating the start of a program file Leader section Used for the title of a program file, etc. Program start Symbol indicating the start of a program Program section Commands for machining Comment section Comments or directions for the operator Tape end Symbol indicating the end of a program file

Tape start

Program section

% TITLE ; O0001 ;

(COMMENT)

Descriptions

Leader section

Program start

Comment section

D Program section

configuration

M30 ; %

Fig. 12 (b) Program configuration

Tape end

A program section consists of several blocks. A program section starts with a program number and ends with a program end code.

Program section Program section configuration

Program number O0001 ; Block 1 N1 G91 G00 X120.0 Y80.0 ; Block 2 N2 G43 Z–32.0 H01 ;

: :

Block n Nn M20 ; Program end M30 ;

A block contains information necessary for machining, such as a move command or coolant on/off command. Specifying a slash (/) at the start of a block disables the execution of some blocks (see ”optional block skip” in 12.2).

B–62574EN/02

PROGRAMMING

12. PROGRAM CONFIGURA TION

12.1

PROGRAM COMPONENTS OTHER THAN PROGRAM SECTIONS

Explanations

D Tape start

This section describes program components other than program sections. See 12.2 for a program section.

Leader section

Tape start

Program section

% TITLE ; O0001 ;

(COMMENT)

M30 ; %

Fig. 12.1(a) Program configuration

Program start

Comment section

Tape end

The tape start indicates the start of a file that contains NC programs. The mark is not required when programs are entered using SYSTEM P or ordinary personal computers. The mark is not displayed on the CRT display screen. However, if the file is output,the mark is automatically output at the start of the file.

D Leader section

D Program start

T able 12.1(a) Code of a tape start

Name

Tape start % ER %

ISO

code

EIA

code

Notation in this manual

Data entered before the programs in a file constitutes a leader section. When machining is started, the label skip state is usually set by turning on the power or resetting the system. In the label skip state, all information is ignored until the first end–of–block code is read. When a file is read into the CNC unit from an I/O device, leader sections are skipped by the label skip function. A leader section generally contains information such as a file header. When a leader section is skipped, even a TV check is not made. So a leader section can contain any codes except the EOB code.

The program start code is to be entered immediately after a leader section, that is, immediately before a program section. This code indicates the start of a program, and is always required to disable the label skip function. With SYSTEM P or ordinary personal computers, this code can be entered by pressing the return key.

Table 12.1(b) Code of a program start

Name ISO

code

Program start LF CR ;

EIA

code

Notation in this manual

12. PROGRAM CONFIGURA TION

PROGRAMMING

B–62574EN/02

NOTE

If one file contains multiple programs, the EOB code for label skip operation must not appear before a second or subsequent program number. However, an program start is required at the start of a program if the preceding program ends with %.

D Comment section

Any information enclosed by the control–out and control–in codes is regarded as a comment.The user can enter a header, comments, directions to the operator, etc. in a comment section using the EOB code or any other code.There is no limit on the length of a comment section.

T able 12.1 (c) Codes of a control–in and a control–out

Name

Control–out ( 2–4–5 ( Start of comment section

Control–in ) 2–4–7 ) End of comment section

ISO

code

EIA

code

Notation in this

manual

Meaning

When a command tape is read into memory for memory operation, comment sections, if any , are not ignored but are also read into memory. Note, however, that codes other than those listed in the code table in Appendix F are ignored, and thus are not read into memory. When data in memory is punched out on paper tape with the punch function, the comment sections are also punched out. When a program is displayed on the screen, its comment sections are also displayed. However, those codes that were ignored when read into memory are not punched out or displayed. During memory operation, all comment sections are ignored. The TV check function can be used for a comment section by setting parameter (No. 0018 #6).

CAUTION

If a long comment section appears in the middle of a program section, a move along an axis may be suspended for a long time because of such a comment section. So a comment section should be placed where movement suspension may occur or no movement is involved.

NOTE

If only a control–in code is read with no matching control–out code, the read control–in code is ignored.

GE Fanuc 0-MD, 0-GSD Operator's Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

SAFETY PRECAUTIONS

GENERAL WARNINGS AND CAUTIONS

WARNINGS AND CAUTIONS RELATED TO PROGRAMMING

WARNINGS AND CAUTIONS RELATED TO HANDLING

WARNINGS RELATED TO DAILY MAINTENANCE

Table of Contents

I. GENERAL

GENERAL

NOTES ON READING THIS MANUAL

GENERAL

PART DRAWING AND TOOL MOVEMENT

Coordinate system

PROGRAM CONFIGURATION

TOOL FIGURE AND TOOL MOTION BY PROGRAM

CONTROLLED AXES

INCREMENT SYSTEM

Maximum stroke

Positioning (G00)

SINGLE DIRECTION POSITIONING (G60)

LINEAR INTERPOLATION (G01)

CIRCULAR INTERPOLATION (G02,G03)

GENERAL

RAPID TRAVERSE

CUTTING FEED

CUTTING FEEDRATE CONTROL

Internal Circular Cutting Feedrate Change

DWELL (G04)

D Reference position

MACHINE COORDINATE SYSTEM

WORKPIECE COORDINATE SYSTEM

Setting a Workpiece Coordinate System

Selecting a Workpiece Coordinate System

LOCAL COORDINATE SYSTEM

PLANE SELECTION

ABSOLUTE AND INCREMENTAL PROGRAMMING (G90, G91)

INCH/METRIC CONVERSION(G20,G21)

DECIMAL POINT PROGRAMMING

TOOL SELECTION FUNCTION

MULTIPLE M COMMANDS IN A SINGLE BLOCK

PROGRAM COMPONENTS OTHER THAN PROGRAM SECTIONS