Content      ..     12      13      14      15     ..

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. OPERATOR'S MANUAL - page 14

3.MANUAL OPERATION

OPERATION

B-64304EN/02

-

Movement in subprogram operation by external subprogram call

In M198 or M-code for subprogram operation by external subprogram call (parameter No.6030), the

backward movement is prohibited though the forward movement is enable.

-

Movement command and M,S,T-code

When M,S,T-codes and movement commands are in the same block, the timing outputting codes changes

between in forward movement and backward movement. Therefore, M, S, T-codes should be commanded

in backward movement after confirming that "DEN" signal is set to "1".

Example of executing the following programs with T series

O0001 ;

M5 S0 F0 ;

G53 X0 Z0 ;

(1)

G1 W100 M3 S100 F1. ;

(2)

G0 U50. W50. ;

(3)

M2 ;

[Forward movement]

(1)G53 X0 Z0

(3) G0 U50. W50.

(2) G1 W100.

M3 S100 F1.

The block of (2) moves with M3 S100 F1.

[Backward movement]

(1)G53 X0 Z0

(3) G0 U50. W50.

(2) G1 W100.

M5 S0 F1.

The block of (2) moves with M5 S0 F1.

-

Non linear interpolation type positioning

In the non-linear interpolation type positioning, the route is different between forward movement and

backward movement.

The route of forward movement

X

The route of backward movement

Z

Please use the interpolation type positioning to ward off danger. (Set the bit 1 (LRP) of parameter

No.1401 to "1") When non linear interpolation type positioning is used, a direction change is prohibited

when any axis stops moving.

- 366 -

B-64304EN/02

OPERATION

4.AUTOMATIC OPERATION

4 AUTOMATIC OPERATION

Programmed operation of a CNC machine tool is referred to as automatic operation.

This chapter explains the following types of automatic operation:

4.1 MEMORY OPERATION

369

Operation by executing a program registered in CNC memory

4.2 MDI OPERATION

371

Operation by executing a program entered from the MDI panel

4.3 DNC OPERATION

374

Function for executing a program while reading the program from an input device connected to the

reader/puncher interface or a memory card.

4.4 SCHEDULE OPERATION

377

Function for executing a program while reading the program from an input device connected to the

reader/puncher interface or a memory card according to a schedule.

4.5 EXTERNAL SUBPROGRAM CALL (M198)

381

Function for calling and executing subprograms (files) registered in an external input/output device

during memory operation

4.6 MANUAL HANDLE INTERRUPTION

383

Function for performing manual feed during movement executed by automatic operation

4.7 MANUAL INTERVENTION AND RETURN

389

Function for making the tool return to its previous position and restarting automatic operation after

movement along an axis has been stopped by feed hold during automatic operation, manual

intervention has been made on the tool, and a request has been made to start automatic operation.

4.8 MIRROR IMAGE

391

Function for enabling mirror-image movement along an axis during automatic operation

4.9 PROGRAM RESTART

392

Restarting a program for automatic operation from an intermediate point

4.1

MEMORY OPERATION

Programs are registered in memory in advance. When one of these programs is selected and the cycle

start switch on the machine operator's panel is pressed, automatic operation starts, and the cycle start LED

goes on.

When the feed hold switch on the machine operator's panel is pressed during automatic operation,

automatic operation is stopped temporarily. When the cycle start switch is pressed again, automatic

operation is restarted.

When the

key on the MDI panel is pressed, automatic operation terminates and the reset state is

entered.

T

For the 2-path control, the programs for the two paths can be executed simultaneously so the two paths

can operate independently at the same time.

The following procedure is given as an example. For actual operation, refer to the manual supplied by the

machine tool builder.

- 369 -

4.AUTOMATIC OPERATION

OPERATION

B-64304EN/02

Memory operation

Procedure

T

1

For the 2-path control, select the path to be operated with the path selection switch on the machine

operator's panel.

2

Press the MEMORY mode selection switch.

3

Select a program from the registered programs. To do this, follow the steps below.

2-1 Press

key to display the program screen.

2-2 Press address

key.

2-3 Enter a program number using the numeric keys.

2-4 Press the [O SRH] soft key.

4

Press the cycle start switch on the machine operator's panel.

Automatic operation starts, and the cycle start LED goes on. When automatic operation terminates,

the cycle start LED goes off.

5

To stop or cancel memory operation midway through, follow the steps below.

a.

Stopping memory operation

Press the feed hold switch on the machine operator's panel. The feed hold LED goes on and

the cycle start LED goes off. The machine responds as follows:

(i)

When the machine was moving, feed operation decelerates and stops.

(ii) When dwell was being performed, dwell is stopped.

(iii) When M, S, or T was being executed, the operation is stopped after M, S, or T is finished.

When the cycle start switch on the machine operator's panel is pressed while the feed hold LED

is on, machine operation restarts.

b.

Terminating memory operation

Press the

key on the MDI panel.

Automatic operation is terminated and the reset state is entered.

When a reset is applied during movement, movement decelerates then stops.

Explanation

-

Memory operation

After memory operation is started, the following are executed:

(1) A one-block command is read from the specified program.

(2) The block command is decoded.

(3) The command execution is started.

(4) The command in the next block is read.

(5) Buffering is executed. That is, the command is decoded to allow immediate execution.

(6) Immediately after the preceding block is executed, execution of the next block can be started. This is

because buffering has been executed.

(7) Hereafter, memory operation can be executed by repeating the steps (4) to (6).

-

Stopping and terminating memory operation

Memory operation can be stopped using one of two methods: Specify a stop command, or press a key on

the machine operator's panel.

• The stop commands include M00 (program stop), M01 (optional stop), and M02 and M30 (program

end).

• There are two keys to stop memory operation: The feed hold key and reset key.

- 370 -

4.AUTOMATIC OPERATION

OPERATION

B-64304EN/02

MDI Operation

Procedure

1

Select the MDI mode.

T

For the 2-path control, select the path for which a program is created and select MDI mode. A

program is created for each path.

2

Press the

key to select the program screen. The following screen appears:

MDI program screen

At this time, program number “O0000” is inserted automatically.

3

Prepare a program to be executed by an operation similar to normal program editing. M99 specified

in the last block can return control to the beginning of the program after operation ends. Word

insertion, modification, deletion, word search, address search, and program search are available for

programs created in the MDI mode.

4

To entirely erase a program created in MDI mode, use one of the following methods:

a.

Enter address

key, then press the

key.

b.

Alternatively, press the

key. In this case, set parameter MCL (No. 3203#7) to 1 in

advance.

5

To execute a program, set the cursor on the head of the program.

Push Cycle Start button on the operator's panel. By this action, the prepared program will start.

When the program end (M02, M30) or EOR(%) is executed, the prepared program will be

automatically erased and the operation will end.

By command of M99, control returns to the head of the prepared program.

6

To stop or terminate MDI operation in midway through, follow the steps below.

a.

Stopping MDI operation

Press the feed hold switch on the machine operator's panel. The feed hold LED goes on and the

cycle start LED goes off. The machine responds as follows:

(i)

When the machine was moving, feed operation decelerates and stops.

(ii) When dwell was being performed, dwell is stopped.

(iii) When M, S, or T was being executed, the operation is stopped after M, S, or T is finished.

When the cycle start switch on the machine operator's panel is pressed, machine operation

restarts.

- 372 -

B-64304EN/02

OPERATION

4.AUTOMATIC OPERATION

b.

Terminating MDI operation

Press the

key.

Automatic operation is terminated and the reset state is entered.

When a reset is applied during movement, movement decelerates then stops.

Explanation

The previous explanation of how to execute and stop memory operation also applies to MDI operation,

except that in MDI operation, M30 does not return control to the beginning of the program (M99

performs this function).

-

Erasing the program

Programs prepared in the MDI mode will be erased in the following cases:

• In MDI operation, if M02, M30 or EOR(%) is executed.

• When bit 6 (MER) of parameter No. 3203 is set to 1, and the last block of the program is executed in

single block operation

NOTE

In the two cases above, program erasure can be prevented by setting bit 6

(MKP) of parameter No. 3204 to 1.

• In MEM mode, if memory operation is performed.

• In EDIT mode, if any editing is performed.

• When the

and

keys are pressed.

• Upon reset when bit 7 (MCL) of parameter No.3203 is set to 1

NOTE

Upon reset when the parameter MCL = 0, the cursor moves to the end of the

program.

-

Restart

If a program is not executed even once after the program is input, the program is executed from the

beginning, regardless of where the cursor is placed. However, a program is executed starting at the

beginning of the block where the cursor is place, if the program is stopped for a reason such as single

block operation after restart of an MDI operation then is restarted after an editing operation.

CAUTION

When an MDI program is restarted, the program is executed starting at the

beginning of the block where the cursor is placed, regardless of the cursor

position in the block.

(Example)

When the cursor is placed on G90

:

G91 X100.0 G90 Y200.0 Z300.0 ;

:

The program is executed starting at the beginning (namely, G91) of this

block. So, the tool moves by 100.0 along the X-axis in the incremental

programming, and moves to 200.0 and 300.0 along the Y-axis and Z-axis,

respectively, in the absolute programming.

-

Editing a program during MDI operation

A program can be edited during MDI operation. By setting bit 5 (MIE) of parameter No. 3203 to 1,

editing can be disabled. However, even when bit 5 (MIE) of parameter No. 3203 is set to 1, editing can

be enabled by resetting the operation.

- 373 -

4.AUTOMATIC OPERATION

OPERATION

B-64304EN/02

-

Absolute/incremental command

When bit 4 (MAB) of parameter No. 3401 is set to 1, the absolute/incremental programming of MDI

operation does not depend on G90/G91. In this case, the incremental programming is set when bit 5

(ABS) of parameter No. 3401 is set to 0, and the absolute programming is set when bit 5 (ABS) of

parameter No. 3401 is set to 1.

Parameter MAB (No.3401#4)=0

Parameter MAB (No.3401#4)=1

Absolute mode operation with G90

Parameter ABS (No.3401#5)=0

Parameter ABS (No.3401#5)=1

command, and incremental

Incremental mode operation at all

Absolute mode operation at all

programming operation with G91

times, independent of G90/G91

times, independent of G90/G91

command

command

command

NOTE

When G code system A is used on a T series, the parameters MAB and ABS are

invalid.

Limitation

-

Program registration

Programs created in MDI mode cannot be registered.

-

Number of characters in a program

A created program can consist of up to 511 characters including "O0000" automatically inserted.

-

Subprogram nesting

The subprogram call command (M98) can be described in a program created in MDI mode. That is,

programs that are registered in memory through MDI operation can be called and executed. The level of

subprogram call nesting is the same as in MEM operation.

-

Macro call

When the custom macro function is enabled (bit 5 (NMC) of parameter No. 8135 is 0), a macro program

can be created and executed even in the MDI mode. Moreover, a macro program can be called for

execution.

NOTE

The GOTO statement, WHILE statement, and DO statement cannot be executed

in a program created in the MDI mode. An alarm PS0377 is issued.

When a program including those statements is to be executed, register the

program in the program memory then call the program for execution.

4.3

DNC OPERATION

By activating automatic operation during the DNC operation mode (RMT), it is possible to perform

machining (DNC operation) while a program is being read in via reader/puncher interface.

To use the DNC operation function, it is necessary to set the parameters related to the reader/punch

interface in advance.

The procedure described below is just an example. For actual operation, refer to the relevant manual of

the machine tool builder.

DNC operation

Procedure

1

Press the REMOTE switch on the machine operator's panel to enter the RMT mode.

- 374 -

B-64304EN/02

OPERATION

4.AUTOMATIC OPERATION

2

Select the program to be executed.

•

Selecting a DNC operation file

Enter the number of the file to be subjected to DNC operation is performed on the memory card

(or floppy cassette) list screen with the keyboard and press soft key [DNC SET] (or [DNC

SET] for the 10.4-inch display unit) to select the file to be subjected to DNC operation.

(The

selected file is marked with "D".)

•

Releasing a DNC operation file

Press soft key [DNC CLR] (or [DNC CLR] for the 10.4-inch display unit) on the memory card

(or floppy cassette) list screen to release the DNC operation file.

(The "D" mark for the file is

removed.)

3

Press the cycle start switch to execute the selected file. For details on the REMOTE switch, refer to

the manual provided by the machine tool builder.

4

During DNC operation, executed programs are listed on the program check screen and program

screen.

Fig. 4.3 (a) PROGRAM screen

- 375 -

4.AUTOMATIC OPERATION

OPERATION

B-64304EN/02

Fig. 4.3 (b) PROGRAM CHECK screen

NOTE

1 Before selecting a DNC operation file, be sure to release all schedule data.

DNC operation and schedule operation cannot be specified at the same time.

2 A DNC operation file cannot be released during DNC operation.

3 To switch between devices when DNC settings are made, release the settings

and then make the settings again.

Explanation

During DNC operation, subprograms and macro programs stored in memory can be called.

Limitation

-

M198 (command for calling a program from within an external input/output

unit)

In DNC operation, M198 cannot be executed. If M198 is executed, alarm PS0210 is issued.

-

Custom macro

In DNC operation, custom macros can be specified, but no repeat instruction and branch instruction can

be programmed. If a repeat instruction or branch instruction is executed, alarm PS0123 is issued.

-

M99

For returning from a subprogram or macro program to the calling program during DNC operation, the

specification of a return command (M99P...) with a sequence number specified is not allowed.

T

-

2-path concurrent operation

DNC operation cannot be performed concurrently on two paths.

DNC operation can be performed on one path at a time.

- 376 -

B-64304EN/02

OPERATION

4.AUTOMATIC OPERATION

4.4

SCHEDULE OPERATION

To perform schedule operation, select files (programs) registered in a memory card and specify the

sequence of execution and the repetition count of each program.

Schedule operation

Procedure

1

Press the REMOTE switch on the machine operator's panel to enter the RMT mode.

2

Select the program to be subjected to schedule operation.

•

Selecting a schedule

Select the file to be subjected to schedule operation. After selecting the file, press soft key

[SCHDL] to display the schedule list screen.

Fig. 4.4 (a) Program list screen (10.4-inch)

[SCHDL]

Lists the settings of schedule data to edit the repetition count or the like (see the next page for

details).

• Setting and editing a schedule (for the 10.4-inch display unit)

Move the cursor to the FILE NUMBER field or FILE NAME field of the desired number, enter the

file number or file name with the keyboard, and press edit key

to schedule the file.

Schedule operation is performed in ascending order of the number. When a schedule is set in this

procedure, the file execution repeat count is set to 1. The repeat count and the order of schedule

operation can be edited on this screen.

- 377 -

4.AUTOMATIC OPERATION

OPERATION

B-64304EN/02

Fig. 4.4 (b) Schedule list screen (10.4-inch)

[FILE UP]

Moves the file at the cursor position up one line and moves the replaced file down one line.

[FILE DOWN]

Moves the file at the cursor position down one line and moves the replaced file up one line.

[DELETE]

Deletes the file at the cursor position and moves the files below the cursor up one line.

[INSERT]

Moves the files below the cursor down one line.

[ALL DELETE]

Deletes all records.

• Setting and editing a schedule (for the 8.4-inch display unit)

There are two schedule list screens for the 8.4-inch display unit: the file number screen for setting

file numbers and the file name screen for setting file names. On the schedule list screen, press

continuous menu key

and press soft key [F-NAME] or [F-NO] to select one of the two screen.

(When the file number screen is displayed, soft key [F-NAME] appears. When the file name

screen is displayed, soft key [F-NO] appears.)

Move the cursor to the FILE NUMBER field or FILE NAME field of the desired number, enter the

file number or file name with the keyboard, and press edit key

to schedule the file. Schedule

operation is performed in ascending order of the number. When a schedule is set in this procedure,

the file execution repeat count is set to 1. The repeat count and the order of schedule operation can

be edited on this screen.

- 378 -

B-64304EN/02

OPERATION

4.AUTOMATIC OPERATION

Fig. 4.4 (c) File number screen (schedule list screen)(8.4-inch)

Fig. 4.4 (d) File name screen (schedule list screen) (8.4-inch display unit)

Fig. 4.4 (e) Soft key [F-NO] (8.4-inch display unit)

Fig. 4.4 (f) Soft key [F-NAME] (8.4-inch display unit)

[F-UP]

Replaces the file at the cursor position with the file located one line above.

[F-DOWN] Replaces the file at the cursor position with the file located one line below.

[DELETE] Deletes the file at the cursor position and moves the files at the lower positions up one

line.

[INST]

Moves the files at the cursor and lower positions down one line.

[ALLDEL] Deletes all records.

[F-NO]

Displays the file number screen.

- 379 -

4.AUTOMATIC OPERATION

OPERATION

B-64304EN/02

[F-NAME] Displays file name screen.

The files registered as schedule data are marked with "S" to the left of their file names on the

program list screen.

Fig. 4.4 (g) Program list screen (after setting schedule data) (10.4-inch display unit)

3

Press the cycle start switch to execute the selected files. For details on the REMOTE switch, refer

to the manual provided by the machine tool builder.

NOTE

1 Before setting schedule operation, release DNC operation files in the MDI mode.

DNC operation and schedule operation cannot be specified at the same time.

2 Before starting schedule operation, confirm that schedule data is set correctly on

the schedule list screen.

3 Schedule data cannot be changed or edited during schedule operation. Before

changing schedule data, make a reset to stop operation.

Restrictions

-

Repetition count

The maximum repetition count during schedule operation is 9999. When a negative value is specified,

an endless loop (LOOP display) is assumed. The file for which 0 is set is skipped and processing

proceeds to the next file.

-

Number of registered files

The maximum number of programs that can be registered as schedule setting data is 20.

-

Selectable files

The files to be selected as schedule setting data must be registered in the same directory.

(Files in the

different directories cannot be selected.)

-

M code

Even if a code other than M02 and M30 in the execution program is executed, the current count on the

schedule execution status screen is not increased.

- 380 -

B-64304EN/02

OPERATION

4.AUTOMATIC OPERATION

-

Floppy disk directory display during execution of a file

During schedule operation, directories in a floppy disk cannot be displayed in a background edit.

-

Intervention during automatic operation

Intervention in schedule operation cannot be performed during automatic operation.

T

-

During 2-path control

The scheduling function cannot be used by two paths at the same time.

4.5

EXTERNAL SUBPROGRAM CALL (M198)

During memory operation, you can call and execute a subprogram registered in an external device (such

as a Memory Card, Handy File, or Data Server) connected to the CNC.

Format

M198 Pxxxxxxxx Lyyyyyyyy ;

↑

↑

Pxxxxxxxx : Program number (or file number)

Lyyyyyyyy : Number of repetitive calls

When address L is omitted, the number of repetitive calls is assumed to be 1.

FS0i-C compatible command format

M198 Pxxxx yyyy ;

↑

↑

xxxx : Number of repetitive calls

yyyy : Program number (or file number)

When the number of repetitive calls is omitted, it is assumed to be 1.

Explanation

M code M198 specifies an external subprogram call. You can also call an external subprogram using an

M code set in parameter No. 6030.

(When an M code other than M198 is set as an M code for calling an

external subprogram, M198 is executed as a normal M code.)

Specify a program number (file number) registered in an external device at address P. If the specified

program number (file number) is not registered in the connected external device, an alarm (PS1079) is

issued.

(When the memory card is used as external device, alarm (SR1966) is issued.)

- 381 -

4.AUTOMATIC OPERATION

OPERATION

B-64304EN/02

Example)

M198 P0123 L3 ;

This command specifies that the subprogram having external subprogram number

O0123 is to be called three times repeatedly.

The subprogram is called from the main program and executed as follows:

Main program

Sub program

1

2

3

N0010 ... ;

0123 ... ;

N0020 ... ;

N1020 ... ;

N0030 M198 P0123 L3 ;

N1030 ... ;

N0040 ... ;

N1040 ... ;

N0050

;

N0050 ... ;

N0060 ... ;

N1060 ... M99 ;

-

Program number call

You can also specify a subprogram call with its program number instead of the file number by the setting

of bit 2 (SBP) of parameter No. 3404.

NOTE

1

An external subprogram call can be specified during program operation in the

MEM mode or MDI mode. To make an external subprogram call in the MDI

mode, set bit 1 (MDE) of parameter No. 11630 to 1.

2

An external subprogram call is available for the following external devices:

External device name

Program number call

File number call

Handy File

Available

Available

FLOPPY CASSTTE

Available

Available

Memory Card

Available

Unavailable

Data Server

Available

Unavailable

3

To perform a subprogram call using a Memory Card as the external device, set

bit 7 (MNC) of parameter No. 138 to 1 and I/O channel (parameter No. 0020) to

4.

A program number call is always enabled regardless of the setting of bit 2 (SBP)

of parameter No. 3404.

4

An external device subprogram call cannot be performed from a subprogram

called using another external device subprogram call.

(An alarm (PS1080) is

issued.)

Main program

Sub program

Sub program

(internal memory)

(External device)

(External device)

Can be called.

Cannot be

called.

M198

M198

(Alarm)

5

A subprogram registered in internal memory can be called from a subprogram

called using an external device subprogram call. From the called subprogram

in internal memory, another external device subprogram call cannot be

performed.

(An alarm (PS1080) is issued.)

Main program

Sub program

Sub program

Sub program

(internal memory)

(External

(internal

(External

device)

memory)

device)

M198

M98

M198

Can be called.

Cannot be called.

Can be called.

(Alarm)

- 382 -

B-64304EN/02

OPERATION

4.AUTOMATIC OPERATION

NOTE

6 A call using the external device subprogram call function is counted as one level

of subprogram nesting.

7 In a 2-path system (T series), an external device subprogram call cannot be

performed simultaneously from both paths.

4.6

MANUAL HANDLE INTERRUPTION

By rotating the manual pulse generator in the automatic operation mode (manual data input, DNC

operation, or memory operation) or in the memory editing mode, handle feed can be superimposed on

movement by automatic operation. A handle interruption axis is selected using the manual handle

interruption axis selection signal.

The minimum unit of travel distance per scale division is the least input increment. One of four types of

magnifiers selected with MP1 and MP2 <G019.4 and 5> can be applied. With bit 3 (HIT) of parameter

No. 7103, the minimum unit of travel distance can be further 10 times greater. A handle feed magnifier

is selected using the manual handle feed amount selection signal.

(See Section III-4.6, "MANUAL

HANDLE FEED".)

Tool position

Programmed

X

during automatic

Tool position after

depth of cut

operation

handle interruption

Depth of cut

by handle

Z

interruption

Workpiece

Fig. 4.6(a) Manual handle interruption

WARNING

The travel distance per scale division by manual handle interruption is the least

input increment as with manual handle feed. For example, in the case of IS-B,

254 ticks correspond to 0.01 inch for a millimeter input/inch output machine and

100 ticks correspond to 0.254 millimeter for an inch input/millimeter output

machine.

Explanation

-

Interruption operation

1

When the handle interruption axis selection signal for a handle interruption axis is set to 1 in the

automatic operation mode (manual data input, DNC operation, or memory operation) or in the

memory editing mode, manual handle interruption can be performed by rotating the handle of the

manual pulse generator.

NOTE

Even when the feedrate override signal sets 0%, manual handle interruption can

be accepted.

2

For the method of selecting a manual handle interruption axis, refer to the relevant manual of the

machine tool builder.

- 383 -

4.AUTOMATIC OPERATION

OPERATION

B-64304EN/02

3

The feedrate during manual handle interruption is the sum of feedrate used for automatic operation

and the feedrate used for movement by manual handle interruption. However, the feedrate during

manual handle interruption is controlled so that it does not exceed the maximum allowable cutting

feedrate for the axis.

Example

Suppose that the maximum allowable cutting feedrate for an axis is 5 m/min, and

that a movement is made in the + direction at 2 m/min along the axis. In this

case, manual handle interruption can be accepted even when the manual pulse

generator is rotated up to a speed equivalent to 3 m/min. Manual handle

interruption by rotation in one direction can be accepted even when the manual

pulse generator is rotated to a speed equivalent to 7 m/min.

If the manual pulse generator is rotated to a speed beyond the upper limits,

those pulses from the manual pulse generator that correspond to the excess are

lost, resulting in a mismatch between the scale mark of the manual pulse

generator and the actually interrupted travel distance.

4

For a magnifier for manual handle interruption, refer to the relevant manual of the machine tool

builder.

5

If the travel direction is reversed as a result of manual handle interruption, backlash compensation is

performed. Pitch error compensation is performed for the position after interruption.

6

In manual handle interruption, only acceleration/deceleration for cutting feed is enabled. By

setting bit 0 (MNJ) of parameter No. 1606 to 1, acceleration/deceleration for both of cutting feed and

jog feed can be applied to manual handle interruption.

-

Manual handle interruption and coordinate system

1

The amount of manual handle interruption shifts the workpiece coordinate systems and the local

coordinate system. So, the machine moves, but the coordinates in the workpiece coordinate

systems and the local coordinate system remain unchanged.

Regardless of which coordinate system is selected, all workpiece coordinate systems and the local

coordinate system shift by the same amount.

•

Absolute coordinates

→ Remain unchanged by handle interruption.

•

Relative coordinates

→ Change by the amount of handle interruption.

•

Machine coordinates

→ Change by the amount of handle interruption.

Programmed path

Path after

interruption

Shift by manual handle

interruption

(Workpiece coordinate system before

interruption)

(Workpiece coordinate system after

interruption)

(Machine coordinate system)

- 384 -

B-64304EN/02

OPERATION

4.AUTOMATIC OPERATION

2

Even when manual handle interruption is performed, the machine coordinate system remains

unchanged. The absolute command (G53) in the machine coordinate system is not affected by

manual handle interruption.

(G90G54****)

Programmed path

Path after

interruption

Shift by manual handle

interruption

(Workpiece coordinate system before

interruption)

(Workpiece coordinate system after

(G90G53****)

interruption)

(Machine coordinate system)

3

In automatic reference position return (G28), the end point (reference position) is not affected by

manual handle interruption. However, the midpoint is in the workpiece coordinate system, so that

the position shifted by the amount of interruption becomes the midpoint.

-

Cancellation of the amount of interruption

Operation by which the workpiece coordinate system shifted by manual handle interruption from the

machine coordinate system is returned to the original workpiece coordinate system is referred to

cancellation of the amount of interruption.

When the amount of interruption is canceled, the workpiece coordinate system is shifted by the amount of

manual handle interruption, and the amount of interruption is reflected in the absolute coordinates.

Interruption shifts the workpiece coordinate system from the machine coordinate system.

Position before interruption

Workpiece

coordinate system

before interruption

Workpiece

origin offset

Interruption

Position after

interruption

Workpiece

coordinate

system after

(Machine zero point)

interruption

- 385 -

4.AUTOMATIC OPERATION

OPERATION

B-64304EN/02

By cancellation, the workpiece coordinate system returns to the state present before handle interruption.

Workpiece

coordinate system

Workpiece

after cancellation

Interruption amount

origin

cancellation

offset

Position after

cancellation

Workpiece

coordinate

system before

cancellation

(Machine zero point)

In the following cases, the amount of interruption is canceled:

• When a reset is made (when bit 1 (RTH) of parameter No. 7103 is set to 1)

• When emergency stop state is canceled (when bit 1 (RTH) of parameter No. 7103 is set to 1)

• When a manual reference position return operation is performed

(when G28 is specified before a reference position is established)

• When a reference position is set without dogs

• When the workpiece coordinate system is preset

NOTE

When the amount of interruption is cleared using soft keys, only the indication of

the amount of interruption becomes 0, and the workpiece coordinate system

remains unchanged.

-

Clearing the amount of interruption by soft keys

Clearing of the amount of interruption means that the indication of the amount of interruption by manual

handle interruption is set to 0. The workpiece coordinate system does not change.

"Clearing all axes" or "Clearing any axis" is performed on the path for which the amount of manual

handle interruption is indicated.

When bit 3 (HLC) of parameter No. 7100 is enabled, soft key [INTRPT CANCEL], which is used for this

operation, appears. When HLC is disabled, soft key [INTRPT CANCEL] does not appear.

To select "Clearing all axes" or "Clearing any axis", follow the procedure below.

1

Press function key

on the MDI panel.

2

Press soft key [HANDLE].

3

Press soft key [(OPRT)].

4

To prepare for "Clearing all axes" or "Clearing any axis", press soft key [CANCEL].

To prepare for "Clearing all axes" or "Clearing any axis", perform one of the following.

• Clearing all axes

Press soft key [CANCEL] and then press soft key [ALL-AX].

- 386 -

B-64304EN/02

OPERATION

4.AUTOMATIC OPERATION

• Clearing any axis (there are the following two methods.)

-

Enter the axis name and then press [INTRPTCANCEL].

-

Press soft key [INTRPTCANCEL], enter the axis name, and press soft key [EXEC].

If an incorrect axis name is entered, a warning message stating "FORMAT ERROR" appears.

-

Relation with other functions

The following table indicates the relation between other functions and the movement by handle

interruption.

Table 4.6(a) Relation between other functions and the movement by handle interruption

Signals

Relation

Machine lock is effective. When machine lock is on, no movement is made due to handle

Machine lock

interruption.

Interlock

Interlock is effective. When interlock is on, no movement is made due to handle interruption.

Mirror image is not effective. Interrupt functions on the plus direction by plus direction command,

Mirror image

even if this signal turns on.

-

Position display

The following table shows the relation between various position display data and the movement by

handle interruption.

Table4.6(b) relation between various position display data and the movement by handle interruption

Signals

Relation

Absolute coordinate value

Handle interruption does not change absolute coordinates.

Relative coordinate value

Relative coordinates are changed by the travel distance specified by handle interruption.

Machine coordinates are changed by the travel distance specified by handle

Machine coordinate value

interruption.

-

Travel distance display

Press the function key

, then press the chapter selection soft key [HNDL]. The move amount by

the handle interruption is displayed. The following 4 kinds of data are displayed concurrently.

Fig. 4.6 (b)

(a) INPUT UNIT:

Handle interruption move amount in input unit system

Indicates the travel distance specified by handle interruption according to the least input increment.

- 387 -

B-64304EN/02

OPERATION

4.AUTOMATIC OPERATION

4.7

MANUAL INTERVENTION AND RETURN

When movement along an axis is stopped by feed hold during automatic operation, manual intervention is

performed to check the cut surface, and a restart is made, then the tool returns to the position where it was

before the intervention and automatic operation is restarted.

Explanation

To enable automatic return and intervention, set bit 0 (MIT) of parameter No. 7001 to be enabled.

The automatic return and intervention sequence is described below.

1. The N1 block cuts a workpiece

Tool

N2

N1

2. The tool is stopped by pressing the feed hold switch in the middle of the N1

block (point A).

N2

N1

Point A

3. After retracting the tool manually to point B, tool movement is restarted.

Point B

N2

Manual

intervention

N1

Point A

4. After automatic return to point A at the dry run feedrate, the remaining move

command of the N1 block is executed.

Point B

Return (non-linear interpolation type positioning)

N2

N1

Point A

- 389 -

4.AUTOMATIC OPERATION

OPERATION

B-64304EN/02

WARNING

Be sure to perform correct intervention according to the machining direction and

workpiece figure. Otherwise, the workpiece, machine, or tool may be broken.

Manual

intervention

Point B

N2

N1

Point A

Return (non-linear interpolation

type positionning)

Point B

N2

N1

Point A

-

Manual absolute on/off

In cases such as when tool movement along an axis is stopped by feed hold during automatic operation so

that manual intervention can be used to replace the tool: When automatic operation is restarted, this

function returns the tool to the position where manual intervention was started.

-

Return feedrate

The return feedrate is a dry run feedrate and jog feedrate override is enabled. When manual rapid

traverse signal RT(G0019.7) is 1, the return feedrate is not a dry run feedrate, but a rapid traverse rate.

-

Return operation

Return operation is performed according to non-linear interpolation type positioning.

-

Single block

If the single block stop switch is on during return operation, the tool stops at the stop position and restarts

movement when the cycle start switch is pressed.

-

Cancellation

When a reset, alarm, or emergency stop occurs during manual intervention or return, the manual

intervention and return function is canceled.

-

MDI mode

The manual intervention and return function is enabled in the MDI mode.

Limitation

-

Enabling and disabling manual intervention and return

This function is enabled only when the automatic operation hold LED is on. When the remaining travel

distance is 0, if a feed hold stop is made and manual intervention is performed, manual intervention and

return is disabled and operation is performed according to the specification of the manual absolute on/off

function.

- 390 -

B-64304EN/02

OPERATION

4.AUTOMATIC OPERATION

-

Offset

When the tool is broken, if the tool is replaced by manual intervention and then processing is restarted

from the midpoint in the interrupted block, a change in the offset is not reflected.

-

Machine lock and mirror image

When performing manual intervention and return, do not apply a machine lock or mirror image.

M

-

Scaling

When performing manual intervention and return, do not apply scaling.

4.8

MIRROR IMAGE

During automatic operation, the mirror image function can be used for movement along an axis. To use

this function, set the mirror image switch to ON on the machine operator's panel, or set the mirror image

setting to ON from the MDI panel.

Y Y-axis mirror image goes on.

Programmed tool

path

Tool path after the

mirror image

function is used

Tool

X

Fig. 4.8 (a) Mirror image

Procedure for mirror image

Procedure

The following procedure is given as an example. For actual operation, refer to the manual supplied by the

machine tool builder.

1

Press the single block switch to stop automatic operation.

When the mirror image function is used from the beginning of operation, this step is omitted.

2

Press the mirror image switch for the target axis on the machine operator's panel.

Alternatively, turn on the mirror image setting by following the steps below:

2-1 Set the MDI mode.

2-2 Press the function key

- 391 -

4.AUTOMATIC OPERATION

OPERATION

B-64304EN/02

2-3 Press the [SETING] soft key for chapter selection to display the setting screen.

Fig. 4.8 (b) Setting screen

2-4 Move the cursor to the mirror image setting position, then set the target axis to 1.

3

Enter an automatic operation mode (memory mode or MDI mode), then press the cycle start button

to start automatic operation.

Explanation

• The mirror image function can also be turned on and off by setting bit 0 (MIRx) of parameter

No.0012 to 1 or 0.

• For the mirror image switches, refer to the manual supplied by the machine tool builder.

Limitation

T

The direction of movement during machine coordinate system setting (G53), the direction of movement

during manual operation, and the direction of movement from an intermediate point to the reference

position during automatic reference position return (G28) cannot be reversed.

M

The direction of movement during machine coordinate system setting (G53), the direction of movement

during manual operation, the direction of movement from an intermediate point to the reference position

during automatic reference position return (G28), the direction of approach during single direction

positioning (G60), and the shift direction in a boring cycle (G76, G87) cannot be reversed.

4.9

PROGRAM RESTART

This function specifies Sequence No. of a block to be restarted when a tool is broken down or when it is

desired to restart machining operation after a day off, and restarts the machining operation from that block.

It can also be used as a high-speed program check function.

There are two restart methods: the P-type method and Q-type method.

- 392 -

B-64304EN/02

OPERATION

4.AUTOMATIC OPERATION

Procedure for program restart by specifying a sequence number

Procedure 1

[P TYPE]

1

Retract the tool and replace it with a new one. When necessary, change the offset.

(Go to step 2.)

[Q TYPE]

1

When power is turned ON or emergency stop is released, perform all necessary operations at that

time, including the reference position return.

2

Move the machine manually to the program starting point (machining start point), and keep the

modal data and coordinate system in the same conditions as at the machining start.

3

If necessary, modify the offset amount.

(Go to step 2.)

- 393 -

4.AUTOMATIC OPERATION

OPERATION

B-64304EN/02

Procedure 2

[COMMON TO P TYPE / Q TYPE]

1

Turn the program restart switch on the machine operator's panel ON.

2

Press

key to display the desired program.

3

Find the program head. Press

key.

4

Enter the sequence number of the block to be restarted, then press the [P TYPE] or [Q TYPE] soft

key.

[Q TYPE]

xxxxx

or

[P TYPE]

Sequence

number

If the same sequence number appears more than once, the location of the target block must be

specified. Specify a frequency and a sequence number.

[Q TYPE]

xxxyyyyy

or

[P TYPE]

Sequence number (The rightmost five digits.)

Frequency

5

The sequence number is searched for, and the program restart screen appears on the LCD display.

Fig. 4.9 (a) Program restart screen

DESTINATION shows the position at which machining is to restart.

DISTANCE TO GO shows the distance from the current tool position to the position where

machining is to restart. A number to the left of each axis name indicates the order of axes

(determined by parameter setting) along which the tool moves to the restart position.

The coordinates and amount of travel for restarting the program can be displayed for up to four axes.

If your system supports five or more axes, pressing the [RSTR] soft key again displays the data for

the fifth and subsequent axes.

M : Up to 35 most recently specified M codes. The maximum number of displayed M codes

differs depending on the size of the display.

With 10.4-inch LCD/MDI panel : Up to 30 M codes

With 8.4-inch LCD/MDI panel : Up to 6 M codes

- 394 -

B-64304EN/02

OPERATION

4.AUTOMATIC OPERATION

T : Two most recently specified T codes

S : Most recently specified S code

B : Most recently specified B code

Codes are displayed in the order in which they are specified. All codes are cleared by a program

restart command or cycle start in the reset state.

6

Turn the program re-start switch OFF. At this time, the figure at the left side of axis name

DISTANCE TO GO blinks.

7

Check the screen for the M, S, T, and B codes to be executed. If they are found, enter the MDI

mode, then execute the M, S, T, and B functions. After execution, restore the previous mode.

These codes are not displayed on the program restart screen.

8

Check that the distance indicated under DISTANCE TO GO is correct. Also check whether there

is the possibility that the tool might hit a workpiece or other objects when it moves to the machining

restart position. If such a possibility exists, move the tool manually to a position from which the

tool can move to the machining restart position without encountering any obstacles.

9

Press the cycle start button. The tool moves to the machining restart position at the dry run feedrate

sequentially along axes in the order specified by parameter No. 7310 settings. Machining is then

restarted.

Procedure for program restart by specifying a block Number

Procedure 1

[P TYPE]

1

Retract the tool and replace it with a new one. When necessary, change the offset.

(Go to step 2.)

[Q TYPE]

1

When power is turned ON or emergency stop is released, perform all necessary operations at that

time, including the reference position return.

2

Move the machine manually to the program starting point (machining start point), and keep the

modal data and coordinate system in the same conditions as at the machining start.

3

If necessary, modify the offset amount.

(Go to step 2.)

Procedure 2

[COMMON TO P TYPE / Q TYPE]

1

Turn the program restart switch on the machine operator's panel ON.

2

Press

key to display the desired program.

3

Find the program head. Press

key.

4

Enter the number of the block to be restarted then press the [P TYPE] or [Q TYPE] soft key. The

block number cannot exceed eight digits.

[Q TYPE]

B

xxxxxxxx

or

[P TYPE]

Block number

- 395 -

Content      ..     12      13      14      15     ..