Content      ..     11      12      13      14     ..

FANUC Series Series 16i-TB, Series 18i-TB, Series 160i-TB, Series 180i-TB. OPERATOR’S MANUAL - page 13

B-63524EN/01

PROGRAMMING

15. CUSTOM MACRO

NOTE

For the status-triggered and edge-triggered schemes, see

Item “Custom macro interrupt signal (UINT)” of Subsec.

16.11.2.

15.11.2

Details of Functions

Explanations

D ubprogram-type

There are two types of custom macro interrupts: Subprogram-type

interrupt and macro-type

interrupts and macro-type interrupts. The interrupt type used is selected

interrupt

by MSB (bit 5 of parameter 6003).

(a) Subprogram-type interrupt

An interrupt program is called as a subprogram. This means that the

levels of local variables remain unchanged before and after the

interrupt. This interrupt is not included in the nesting level of

subprogram calls.

(b) Macro-type interrupt

An interrupt program is called as a custom macro. This means that

the levels of local variables change before and after the interrupt. The

interrupt is not included in the nesting level of custom macro calls.

When a subprogram call or a custom macro call is performed within

the interrupt program, this call is included in the nesting level of

subprogram calls or custom macro calls. Arguments cannot be passed

from the current program even when the custom macro interrupt is a

macro-type interrupt.

D M codes for custom

In general, custom macro interrupts are controlled by M96 and M97.

macro interrupt control

However, these M codes, may already being used for other purposes (such

as an M function or macro M code call) by some machine tool builders.

For this reason, MPR (bit 4 of parameter 6003) is provided to set M codes

for custom macro interrupt control.

When specifying this parameter to use the custom macro interrupt control

M codes set by parameters, set parameters 6033 and 6034 as follows:

Set the M code to enable custom macro interrupts in parameter 6033, and

set the M code to disable custom macro interrupts in parameter 6034.

When specifying that parameter-set M codes are not used, M96 and M97

are used as the custom macro control M codes regardless of the settings

of parameters 6033 and 6034.

The M codes used for custom macro interrupt control are processed

internally (they are not output to external units). However, in terms of

program compatibility, it is undesirable to use M codes other than M96

and M97 to control custom macro interrupts.

D Custom macro interrupts

When performing a custom macro interrupt, the user may want to

and NC statements

interrupt the NC statement being executed, or the user may not want to

perform the interrupt until the execution of the current block is completed.

MIN (bit 2 of parameter 6003) is used to select whether to perform

interrupts even in the middle of a block or to wait until the end of the

block.

339

15. CUSTOM MACRO

PROGRAMMING

B-63524EN/01

S

Type I

(i) When the interrupt signal (UINT) is input, any movement or dwell

(when an interrupt is

being performed is stopped immediately and the interrupt program is

performed even in the

executed.

middle of the block)

(ii) If there are NC statements in the interrupt program, the command in

the interrupted block is lost and the NC statement in the interrupt

program is executed. When control is returned to the interrupted

program, the program is restarted from the next block after the

interrupted block.

(iii)If there are no NC statements in the interrupt program, control is

returned to the interrupted program by M99, then the program is

restarted from the command in the interrupted block.

Interrupted by macro interrupt

Execution in

progress

ÉÉÉÉ

ÉÉÉÉ

Normal program

ÉÉÉÉ

CNC command restart; when

there are no NC statements

Interrupt signal (UINT) input

in the interrupt program

Execution in

progress

Custom macro

interrupt

S

Type II

(i)

If the block being executed is not a block that consists of several cycle

(when an interrupt is

operations such as a drilling canned cycle and automatic reference

performed at the end of

position return (G28), an interrupt is performed as follows:

the block)

When an interrupt signal (UINT) is input, macro statements in the

interrupt program are executed immediately unless an NC statement

is encountered in the interrupt program. NC statements are not

executed until the current block is completed.

(ii)

If the block being executed consists of several cycle operations, an

interrupt is performed as follows:

When the last movement in the cycle operations is started, macro

statements in the interrupt program are executed unless an NC

statement is encountered. NC statements are executed after all cycle

operations are completed.

Execution in

progress

Normal program

Interrupt signal (UINT) input

Execution in

progress

ÉÉÉ

Custom macro

ÉÉÉ

NC statement in the

interrupt

interrupt program

340

15. CUSTOM MACRO

PROGRAMMING

B-63524EN/01

D Custom macro interrupt

There are two schemes for custom macro interrupt signal (UINT) input:

signal (UINT)

The status-triggered scheme and edge- triggered scheme. When the

status-triggered scheme is used, the signal is valid when it is on. When

the edge triggered scheme is used, the signal becomes valid on the rising

edge when it switches from off to on status.

One of the two schemes is selected with TSE (bit 3 of parameter 6003).

When the status-triggered scheme is selected by this parameter, a custom

macro interrupt is generated if the interrupt signal (UINT) is on at the time

the signal becomes valid. By keeping the interrupt signal (UINT) on, the

interrupt program can be executed repeatedly.

When the edge-triggered scheme is selected, the interrupt signal (UINT)

becomes valid only on its rising edge. Therefore, the interrupt program

is executed only momentarily (in cases when the program consists of only

macro statements). When the status-triggered scheme is inappropriate,

or when a custom macro interrupt is to be performed just once for the

entire program (in this case, the interrupt signal may be kept on), the

edge-triggered scheme is useful.

Except for the specific applications mentioned above, use of either

scheme results in the same effects. The time from signal input until a

custom macro interrupt is executed does not vary between the two

schemes.

1

0

Interrupt signal (UINT)

Interrupt Interrupt Interrupt

Interrupt

execution execution execution

execution

Status-triggered

scheme

Interrupt

execution

Edge-triggered

scheme

In the above example, an interrupt is executed four times when the status

triggered scheme is used; when the edge- triggered scheme is used, the

interrupt is executed just once.

342

B-63524EN/01

PROGRAMMING

15. CUSTOM MACRO

D Return from a custom

To return control from a custom macro interrupt to the interrupted

macro interrupt

program, specify M99. A sequence number in the interrupted program

can also be specified using address P. If this is specified, the program is

searched from the beginning for the specified sequence number. Control

is returned to the first sequence number found.

When a custom macro interrupt program is being executed, no interrupts

are generated. To enable another interrupt, execute M99. When M99 is

specified alone, it is executed before the preceding commands terminate.

Therefore, a custom macro interrupt is enabled for the last command of

the interrupt program. If this is inconvenient, custom macro interrupts

should be controlled by specifying M96 and M97 in the program.

When a custom macro interrupt is being executed, no other custom macro

interrupts are generated; when an interrupt is generated, additional

interrupts are inhibited automatically. Executing M99 makes it possible

for another custom macro interrupt to occur. M99 specified alone in a

block is executed before the previous block terminates. In the following

example, an interrupt is enabled for the Gxx block of O1234. When the

signal is input, O1234 is executed again. O5678 is controlled by M96 and

M97. In this case, an interrupt is not enabled for O5678 (enabled after

control is returned to O1000).

O1000;

M96P1234;

Interrupt

Interrupt

O1234

GxxXxxx;

M99;

M96P5678

O5678

M97

Interrupt

×

GxxXxxx;

Interrupt

M96;

M99;

M97

NOTE

When an M99 block consists only of address O, N, P, L, or

M, this block is regarded as belonging to the previous block

in the program. Therefore, a single-block stop does not

occur for this block. In terms of programming, the following

(1) and (2) are basically the same.

(The difference is

whether Gff is executed before M99 is recognized.)

(1) Gff Xfff ;

M99 ;

(2) Gff Xfff M99 ;

343

15. CUSTOM MACRO

PROGRAMMING

B-63524EN/01

D Custom macro interrupt

A custom macro interrupt is different from a normal program call. It is

and modal information

initiated by an interrupt signal (UINT) during program execution. In

general, any modifications of modal information made by the interrupt

program should not affect the interrupted program.

For this reason, even when modal information is modified by the interrupt

program, the modal information before the interrupt is restored when

control is returned to the interrupted program by M99.

When control is returned from the interrupt program to the interrupted

program by M99 Pxxxx, modal information can again be controlled by

the program. In this case, the new continuous information modified by

the interrupt program is passed to the interrupted program. Restoration

of the old modal information present before the interrupt is not desirable.

This is because after control is returned, some programs may operate

differently depending on the modal information present before the

interrupt. In this case, the following measures are applicable:

(1) The interrupt program provides modal information to be used after

control is returned to the interrupted program.

(2) After control is returned to the interrupted program, modal

information is specified again as necessary.

O∆∆∆∆

Interrupt signal (UINT)

M96Pxxx

Oxxx;

Modify modal information

(Without P specification)

Modal

information remains

M99(Pffff);

unchanged before and

after the interrupt.

(With P specification)

Nffff;

The new modal information modified by the inter-

rupt program is present.

S Modal information

The modal information present before the interrupt becomes valid. The

when control is

new modal information modified by the interrupt program is made

returned by M99

invalid.

S Modal information

The new modal information modified by the interrupt program remains

when control is

valid even after control is returned. The old modal information which was

returned by M99

valid in the interrupted block can be read using custom macro system

Pffff

variables #4001 to #4120.

Note that when modal information is modified by the interrupt program,

system variables #4001 to #4120 are not changed.

344

B-63524EN/01

PROGRAMMING

15. CUSTOM MACRO

D System variables

D The coordinates of point A can be read using system variables #5001

(position information

and up until the first NC statement is encountered.

values) for the interrupt

D The coordinates of point A′ can be read after an NC statement with no

program

move specifications appears.

D The machine coordinates and workpiece coordinates of point B′ can

be read using system variables #5021 and up and #5041 and up.

Tool nose center path

Interrupt generated

B

B′

A

A′

Offset vector

Programmed tool path

D Custom macro interrupt

When the interrupt signal (UINT) is input and an interrupt program is

and custom macro

called, the custom macro modal call is canceled (G67). However, when

modal call

G66 is specified in the interrupt program, the custom macro modal call

becomes valid. When control is returned from the interrupt program by

M99, the modal call is restored to the state it was in before the interrupt

was generated. When control is returned by M99Pxxxx;, the modal call

in the interrupt program remains valid.

D Custom macro interrupt

When the interrupt signal (UINT) is input while a return operation is being

and program restart

performed in the dry run mode after the search operation for program

restart, the interrupt program is called after restart operation terminates

for all axes. This means that interrupt type II is used regardless of the

parameter setting.

D DNC operation and

“Interruption type custom macro” cannot be done during DNC operation

Interruption type custom

or executing a program with an external input-output device.

macro

345

16. PROGRAMMABLE PARAMETER

B-63524EN/01

PROGRAMMING

ENTRY (G10)

Format

Format

G10L50; Parameter entry mode setting

N_R_; For parameters other than the axis type

N_P_R_; For axis type parameters

G11;

Parameter entry mode cancel

Meaning of command

N_:

Parameter No. (4digits) or compensation position No.(0 to

1023) for

pitch errors compensation +10,000 (5digit)

R_:

Parameter setting value (Leading zeros can be omitted.)

P_:

Axis No. 1 to 8 (Used for entering axis type parameters)

Explanations

D Parameter setting value

Do not use a decimal point in a value set in a parameter (R_).

(R_)

a decimal point cannot be used in a custom macro variable for R_ either.

D Axis No. (P_)

Specify an axis number (P_) from 1 to 8 (up to eight axes) for an axis type

parameter. The control axes are numbered in the order in which they are

displayed on the CNC display.

For example, specify P2 for the control axis which is displayed second.

WARNING

1

Do not fail to perform reference point return manually after

changing the pitch error compensation data or backlash

compensation data. Without this, the machine position can

deviate from the correct position.

2

The canned-cycle mode must be cancelled before entering

of parameters. When not cancelled, the drilling motion will

be activated.

NOTE

Other NC statements cannot be specified while in

parameter input mode.

347

16. PROGRAMMABLE PARAMETER

ENTRY (G10)

PROGRAMMING

B-63524EN/01

Examples

1. Set bit 2 (SPB) of bit type parameter No. 3404

G10L50 ;

Parameter entry mode

N3404 R 00000100 ;

SBP setting

G11 ;

cancel parameter entry mode

2. Change the values for the Z-axis (2nd axis) and C-axis (4th axis) in

axis type parameter No. 1322 (the coordinates of stored stroke limit

2 in the positive direction for each axis).

G10L50 ;

Parameter entry mode

N1322P2R4500 ;

Modify Z axis

N1322P4R12000 ;

Modify C axis

G11 ;

cancel parameter entry mode

348

17. MEMORY OPERATION BY

B-63524EN/01

PROGRAMMING

Series 15 TAPE FORMAT

MEMORY OPERATION BY Series 15 TAPE FORMAT

17

Programs in the Series 15 tape format can be registered in memory for

memory operation by setting bit 1 of parameter No. 0001. Registration

to memory and memory operation are possible for the functions which use

the same tape format as that for the Series 15 as well as for the following

functions which use a different tape format:

• Equal-lead threading

• Subprogram calling

• Canned cycle

• Multiple repetitive canned cycle

• Canned drilling cycle

NOTE

Registration to memory and memory operation are possible

only for the functions available in this CNC.

349

17. MEMORY OPERATION BY

B-63524EN/01

PROGRAMMING

Series 15 TAPE FORMAT

17.2

EQUAL-LEAD

THREADING

Format

G32IP_F_Q_;

or

G32IP_E_Q_;

I

:Combination of axis addresses

P

F :Lead along the longitudinal axis

E :Lead along the longitudinal axis

Q :Sight of the threading start angle

Explanations

D Address

Although the Series 15 allows the operator to specify the number of

threads per inch with address E, the Series 15 tape format does not.

Addresses E and F are used in the same way for specifying the lead along

the longitudinal axis. The thread lead specified with address E is therefore

also assumed as a continuous-state value for address F.

D Specifiable value range

for the thread lead

Address for thread lead

mm input

inch input

0.000001 to

E

0.0001 to 500.0000 mm

9.999999 inch

Command with a

0.000001 to

0.0001 to 500.0000 mm

decimal point

9.999999 inch

F

Command without a

0.01 to 500.00 mm

0.0001 to 9.9999 inch

decimal point

D Specifiable value range

for the feedrate

Address for feedrate

mm input

inch input

Increment

1 to 240000

0.01 to 9600.00

Feed

system (IS-B)

mm/min

inch/min

per

minute

Increment

1 to 100000

0.01 to 4800.00

F

system (IS-C)

mm/min

inch/min

0.01 to 500.00

0.0001 to 9.9999

Feed per rotation

mm/rev

inch/rev

WARNING

Specify the feedrate one more time when switching

between feed per minute and feed per rotation.

351

17. MEMORY OPERATION BY

Series 15 TAPE FORMAT

PROGRAMMING

B-63524EN/01

17.3

SUBPROGRAM

CALLING

Format

M98PffffLffff;

P:Subprogram number

L:Repetition count

Explanation

D Address

Address L cannot be used in this CNC tape format but can be used in the

Series 15 tape format.

The specifiable value range is the same as that for this CNC (1 to 9999).

D Subprogram number

If a value of more than four digits is specified, the last four digits are

assumed as the subprogram number.

D Repetition count

The repetition count L can be specified in the range from 1 to 9999. If no

repetition count is specified, 1 is assumed.

352

17. MEMORY OPERATION BY

B-63524EN/01

PROGRAMMING

Series 15 TAPE FORMAT

17.4

CANNED CYCLE

Format

Outer / inner surface turning cycle (straight cutting cycle)

G90X_Z_F_;

Outer / inner surface turning cycle (taper cutting cycle)

G90X_Z_I_F_;

I:Length of the taper section along the X-axis (radius)

Threading cycle (straight threading cycle)

G92X_Z_F_Q_;

F:Thread lead

Q:Shift of the threading start angle

Threading cycle (taper threading cycle)

G92X_Z_I_F_;

I:Length of the taper section along the X-axis (radius)

End surface turning cycle (front taper cutting cycle)

G94X_Z_F_;

End surface turning cycle (front taper cutting cycle)

G94X_Z_K_F_;

K:Length of the taper section along the Z-axis

D Address

Addresses I and K cannot be used for a canned cycle in this CNC tape

format but can be used in the Series 15 tape format.

D Specifiable value range

Same as that for equal-lead threading in section II-17.2. See section

for the feedrate

II-17.2.

353

17. MEMORY OPERATION BY

Series 15 TAPE FORMAT

PROGRAMMING

B-63524EN/01

17.6

CANNED DRILLING

CYCLE FORMATS

Format

Drilling cycle

G81X_C_Z_F_L_ ; or G82X_C_Z_R_F_L_ ;

R : Distance from the initial level to the R position

P : Dwell time at the bottom of the hole

F : Cutting feedrate

L : Number of repetitions

Peck drilling cycle

G81X_C_Z_R_Q_P_F_L_ ;

R : Distance from the initial level to the R position

Q: Depth of cut in each cycle

P : Dwell time at the bottom of the hole

F : Cutting feedrate

L : Number of repetitions

High-speed peck drilling cycle

G83.1X_C_Z_R_Q_P_F_L_ ;

R : Distance from the initial level to the R position

Q: Depth of cut in each cycle

P : Dwell time at the bottom of the hole

F : Cutting feedrate

L : Number of repetitions

Tapping

G84X_C_Z_R_P_F_L_ ;

R : Distance from the initial level to the R position

P : Dwell time at the bottom of the hole

F : Cutting feedrate

L : Number of repetitions

Rigid tapping

G84.2X_C_Z_R_P_F_L_S_ ;

R : Distance from the initial level to the R position

P : Dwell time at the bottom of the hole

F : Cutting feedrate

L : Number of repetitions

S : Spindle speed

Boring cycle

G85X_C_Z_R_F_L_ ; or G89X_C_Z_R_P_F_L_ ;

R : Distance from the initial level to the R position

P : Dwell time at the bottom of the hole

F : Cutting feedrate

L : Number of repetitions

Cancel

G80 ;

Explanations

D Address

For this CNC tape format, the address used to specify the number of

repetitions is K. For the Series 15 tape format, it is L.

356

17. MEMORY OPERATION BY

B-63524EN/01

PROGRAMMING

Series 15 TAPE FORMAT

D G code

Some G codes are valid only for this CNC tape format or Series 15 tape

format. Specifying an invalid G code results in P/S alarm No. 10 being

generated.

G codes valid only for the Series 15 tape format

G81, G82, G83.1, G84.2

G codes valid only for the Series 16/18/160/180

G87, G88

tape format

D Positioning plane and

For this CNC tape format, the positioning plane and drilling axis are

drilling axis

determined according to the G code for the canned cycle used.

For the Series 15 tape format, the positioning plane and drilling axis are

determined according to G17/G19.

The drilling axis is the basic axis (Z-axis or X-axis) that does not lie in

the positioning plane.

G code

Positioning plane

Drilling axis

G17

XY plane

Z-axis

G19

YZ plane

X-axis

Resetting bit 1 (FXY) of parameter No. 5101 enables fixing of the drilling

axis to the Z-axis.

D Details of data

Data for the canned cycle is specified as follows:

specifying machining

Gjj X C Z R Q P F L

;

Drilling mode

Drilling data

Number of repetitions

Hole position data

Setting

Address

Explanation

Drilling

Gjj

Canned drilling cycle G code

mode

Hole posi-

X/U (Z/W)

Incremental or absolute value used to specify the

tion data

C/H

hole position

Incremental or absolute value used to specify the

Z/W (X/U)

distance from the R position to the bottom of the

hole

Incremental value used to specify the distance

from the initial level to the R position, or absolute

R

value used to specify the R position. Which to use

depends on bit 6 of parameter No. 5102 and the G

Drilling

code system being used.

mode

Incremental value used to specify the depth of cut

Q

in each G83 or G83.1 cycle with radius program-

ming.

Dwell time at the bottom of the hole. The relation-

P

ship between the dwell time and the specified val-

ue is the same as that for G04.

F

Cutting feedrate

Number of repetitions for a sequence of cutting

Number of

L

operations. If L is not specified, it is assumed to

repetitions

be 1.

357

17. MEMORY OPERATION BY

Series 15 TAPE FORMAT

PROGRAMMING

B-63524EN/01

The R position is specified as an incremental value for the distance

D Specifying the R position

between the initial level to the R position. For the Series 15 tape format,

the parameter and the G code system used determine whether an

incremental or absolute value is to be used to specify the distance between

the initial level and the R position.

If bit 6 (RAB) of parameter No. 5102 is 0, an incremental value is always

used. If it is 1, the type of value used depends on the G code system used.

When G code system A is used, an absolute value is used. When G code

system B or C is used, an absolute value is used in G90 mode, and an

incremental value is used in G91 mode.

Series

Series 15 tape format

16/18/160/180

tape format

Bit 6 of parameter

Bit 6 of parameter No. 5102 = 1

No. 5102 = 0

G code system

Incremental

A

B, C

Incremental

G90

G91

Absolute

Absolute

Incremental

D Details of the canned

The correspondence between the G codes and this CNC tape format or

cycle

Series 15 tape format is listed below. This list also provides notes on

dwell during a canned cycle.

No. Gjj (Use) This CNC command format

1. G81 (Drilling cycle)G83 (G87) P0 <Q not specified>

No dwelling

2. G82 (Drilling cycle)G83 (G87) P <Q not specified>

The tool always dwells at the bottom of the hole.

3. G83 (Peck drilling cycle) G83 (G87) <Type B>

If the block contains a P command, the tool dwells at the bottom of the

hole.

4. G83.1 (Peck drilling cycle) G83 (G87) <Type A>

If the block contains a P command, the tool dwells at the bottom of the

hole.

Note) Either type A or B is selected according to bit 2 (RTR) of

parameter No. 5101.

5. G84 (Tapping) G84 (G88)I

f the block contains a P command, the tool dwells after it reaches the

bottom of the hole and after it is retracted to the R position.

6. G84.2 (Rigid tapping) M29 S_ G84 (G88)

If the block contains a P command, the tool dwells before the spindle

starts rotating in reverse at the bottom of the hole and before it starts

rotating in the normal direction at the R position.

7. G85 (Boring cycle) G85 (G89) P0

No dwelling

8. G89 (Boring cycle) G85 (G89) P_

The tool always dwells at the bottom of the hole.

D Clearance d for G83 and

Parameter No. 5114 determines clearance d for G83 and G83.1.

G83.1

358

17. MEMORY OPERATION BY

B-63524EN/01

PROGRAMMING

Series 15 TAPE FORMAT

D Dwell with G83 and

For Series 15-T, G83 or G83.1 does not cause the tool to dwell. For the

G83.1

Series 15 tape format, the tool dwells at the bottom of the hole only if the

block contains a P address.

D Dwelling with G84 and

In Series 15-T, G84/G84.2 causes the tool to dwell before the spindle

G84.2

starts rotating in either the normal or reverse direction, according to the

corresponding parameter setting. For the Series 15 tape format, when the

block contains a P address, the tool dwells at the bottom of the hole and

at the R position before the spindle starts rotating either in the normal or

reverse direction.

D Rigid tapping

For the Series 15 tape format, rigid tapping can be specified by using the

methods listed below:

Format

Condition (parameter), comment

G84.2 X_ Z_ R_ ...S**** ;

Setting (F10/F11) = 1

S**** ;

G84.2 X_ Z_ R_

;

M29 S**** ;

G84 X_ Z_ R_

;

* Common to Series 16 format

M29 S**** G84 X_ Z_ R_

;

G84 X_ Z_ R_

S**** ;

G84 is made a G code for rigid tapping.

Bit 0 (G84) of parameter No. 5200 = 1

S**** ;

G84 X_ Z_ R_

;

* Common to Series 16 format

D Diameter or radius

Specifying 1 for bit 7 (RDI) of parameter No. 5102 causes the canned

programming

cycle R command diameter or radius programming mode in the Series 15

tape format to match the diameter or radius programming mode for the

drilling axis.

D Disabling the Series 15

Specifying bit 3 (F16) of parameter No. 5102 disables the Series 15 tape

format

format. This applies only to the canned drilling cycle. However, the

number of repetitions must be specified by using the L address.

CAUTION

Setting bit 3 (F16) of parameter No. 5102 to 1 overrides bits

6 (RAB) and 7 (RDI) of parameter No. 5102; both settings

are assumed to be 0.

Limitations

D C-axis as the drilling

It is impossible to use the C-axis (the third axis) as a drilling axis. So,

axis

specifying G18 (ZX plane) generates P/S alarm No. 28 (plane selection

command error).

D Clamping the C-axis

For the Series 15 tape format, it is impossible to specify an M code for

clamping the C-axis.

359

18. FUNCTIONS FOR HIGH SPEED

B-63524EN/01

PROGRAMMING

CUTTING

This function can convert the machining profile to a data group that can

18.1

be distributed as pulses at high-speed by the macro compiler and macro

HIGH SPEED CYCLE

executor. The function can also call and execute the data group as a

CUTTING

machining cycle using the CNC command (G05 command).

This function is applied to 1-path lathe control.

Format

G05 P10fff Lfff ;

P10fff is number of the machining cycle to be called first:

P10001 to P10999

Lfff is repetition count of the machining cycle

(L1 applies when this parameter is omitted.) :

L1 to L999

Call and execute the data for the high speed cutting cycle specified by the

macro compiler and macro executor using the above command.

Cycle data can be prepared for up to 999 cycles. Select the machining

cycle by address P. More than one cycle can be called and executed in

series using the cycle connection data in the header.

Specify the repetition count of the called machining cycle by address L.

The repetition count in the header can be specified for each cycle.

The connection of cycles and their repetition count are explained below

with an example.

Example) Assume the following:

Cycle 1 Cycle connection data 2 Repetition count 1

Cycle 2 Cycle connection data 3 Repetition count 3

Cycle 3 Cycle connection data 0 Repetition count 1

G05 P10001 L2 ;

The following cycles are executed in sequence:

Cycles 1, 2, 2, 2, 3, 1, 2, 2, 2, and3

NOTE

1

An alarm is issued if the function is executed in the G41/G42

mode.

2

Single block stop, dry run/feedrate override, automatic

acceleration/deceleration and handle interruption are

disabled during high-speed cycle machining.

361

18. FUNCTIONS FOR HIGH SPEED

CUTTING

PROGRAMMING

B-63524EN/01

Alarms

Alarm

Descriptions

number

115

The contents of the header are invalid. This alarm is issued in

the following cases.

1. The header corresponding to the number of the specified

call machining cycle was not found.

2. A cycle connection data value is not in the valid range

(0 to 999).

3. The number of data items in the header is not in the valid

range (1 to 32767).

4. The first variable No. for storing data in the executable

format is not in the valid range (#20000 to #85535).

5. The last variable No. for storing data in the executable

format exceeds the limit (#85535).

6. The first variable No. for start data in the executable

format overlaps with a variable No. used in the header.

178

High-speed cycle machining was specified in the G41/G42

mode.

179

The number of control axes specified in parameter 7510 ex-

ceeds the maximum number.

362

18. FUNCTIONS FOR HIGH SPEED

B-63524EN/01

PROGRAMMING

CUTTING

During high-speed machining, the distribution processing status is

18.2

monitored. When distribution processing terminates, P/S alarm No. 000

DISTRIBUTION

and P/S alarm No. 179 are issued upon completion of the high-speed

PROCESSING

machining command (according to the setting of ITPDL (bit 7 of

TERMINATION

parameter No. 7501)).

MONITORING

These P/S alarms can be canceled only by turning off the CNC power.

FUNCTION FOR THE

HIGH-SPEED

MACHINING

COMMAND (G05)

Explanations

D High-speed machining

High-speed machining using the high-speed remote buffer A function,

command

high-speed remote buffer B function, and high-speed cycle function

based on the G05 command

D Distribution processing

Failure to perform normal distribution processing because distribution

termination

processing required for high-speed machining exceeded the CNC

processing capacity, or because distribution data sent from the host was

delayed for some reason while the high-speed remote buffer A or G

function was being used

Number

Message

Contents

000

PLEASE TURN OFF POWER

During high-speed machining,

distribution processing was ter-

minated.

Related parameters:

Remote buffer transfer baud rate

(parameter No. 133)

179

PARAM. (NO. 7510) SETTING

Number of controlled axes in

ERROR

high-speed machining (parame-

ter No. 7150)

High-speed axis selection dur-

ing high-speed machining (bit 0

of parameter No. 7510)

363

18. FUNCTIONS FOR HIGH SPEED

B-63524EN/01

PROGRAMMING

CUTTING

Notes

NOTE

1

If a block without a move command is encountered in the

advanced preview control mode, the tool decelerates and

stops in the previous block.

2

If a move block in the advanced preview control mode

contains an M, S, or T code, the tool decelerates and stops

in that block.

3

If a one-shot G code such as G04 is specified in the

advanced preview control mode, the tool decelerates and

stops in the previous block.

4

If an axial machine lock signal (MLK1 to MLK8) is set on or off

in the advanced preview control mode, acceleration/

deceleration is not carried out on the axis on which the

machine lock is performed.

5

The automatic corner override in the advanced preview

control mode can change just the internal arc cutting speed.

6

If an overtravel alarm occurs in the advanced preview

control mode, the tool decelerates and stops after the alarm

occurs. That is, the tool overruns by the deceleration

distance.

7

If the feed per revolution command is specified in the

advanced preview control mode, the spindle speed can be

changed up to 30000 min^-1.

8

If a feed per minute block is followed or preceded by a feed

per revolution block in the advanced preview control mode,

the tool decelerates and stops in the previous block.

Limitations

D G08 command

Specify G08 code only in a block.

D Threading

Because this function involves automatic velocity control, the tool

decelerates in a corner, automatically changing the depth of cut, even in the

feed per minute mode. Therefore, this function cannot be used for threading.

Automatic deceleration is performed also in the feed per revolution mode.

D Functions that cannot be

In the advanced preview control mode, some functions cannot be specified.

specified in the

When specifying any of those functions, cancel the advanced preview

advanced preview

control mode in advance. After specifying the function, select the advanced

control mode

preview control mode again. The table below indicates the applicability of

the functions.

Function name

Applicability

Canned cycle for grinding

Y

Hypothetical axis interpolation

Y

8-digit program number preceded by O

f

Rapid traverse bell-shaped acceleration/deceleration

f

Dual position feedback

f

365

18. FUNCTIONS FOR HIGH SPEED

CUTTING

PROGRAMMING

B-63524EN/01

Function name

Applicability

Learning function

Y

Look-ahead repetition control

Y

Polygon between spindles

Y

Abnormal load detect function

f

Chuck/tailstock barrier

Y

PMC axis control velocity command function

Y

Corner rounding

f

Butt-type reference position setting

f

Circular threading

Y

Tandem control

f

C executor + macro executor

f

Motor velocity signal output

f

Additional C executor memory

f

Two Floppy Cassette control

f

Main CPU custom software capacity

f

Sub CPU custom software capacity

f

Straightness compensation

f

Simple spindle synchronization

f

Stroke limit check before movement

Y

Manual linear/circular interpolation

f

Three/four spindle serial outputs

f

Third/fourth spindle orientation

f

Third/fourth spindle output selection

f

Controlled axis count specification (sub side)

f

Controlled axis expansion

f

Controlled axis count specification

f

Simultaneous controlled axis expansion

f

Axis control by PMC

Y (*1)

Increment system 1/10

f

Linear acceleration/deceleration after cutting feed in-

f

terpolation

Axis removal

f

Feedrate second override

f

366

18. FUNCTIONS FOR HIGH SPEED

B-63524EN/01

PROGRAMMING

CUTTING

Function name

Applicability

Linear acceleration/deceleration before cutting feed

f

interpolation

Polar coordinate interpolation

Y

Cylindrical interpolation

Y

Polygon turning

Y

Helical interpolation

f

Tool retract & return

Y

Threading retract

Y

Continuous threading

Y

Variable-lead threading

Y

Rigid tapping

Y

Bell-shaped acceleration/deceleration after cutting

f

feed interpolation

Third/fourth reference position return

f

Floating reference position return

f

High-speed cycle cutting

Y

Axis recomposition

Y

Balance cut

Y

Single manual handle control

f

Double manual handle control

f

Handle interrupt

Y

Program restart

Y

Tool post interference check

Y

Expanded stored stroke check

Y

Stored pitch error compensation

f

External deceleration

f

Simple synchronization control

Y

Sequence number collation stop

f

Position switch

Y

Feed stop

Y

High-speed skip function

Y

Multistage skip function

Y

S serial output

f

Spindle positioning

Y

367

18. FUNCTIONS FOR HIGH SPEED

CUTTING

PROGRAMMING

B-63524EN/01

Function name

Applicability

Cs contour control

Y (*2)

First spindle orientation

f

First spindle output selection

f

Constant surface speed control

f

Actual spindle speed output

f

Spindle speed fluctuation detection

f

Spindle synchronization control

f

Multi-spindle control

f

S analog output

f

Second spindle orientation

f

Second spindle output selection

f

Direct drawing dimension programming

f

Special G code

f

Programmable data input

f

Custom macro B

f

Interrupt-type custom macro

Y

Chamfer, corner rounding

f

Inch/metric selection

f

Multiple repetitive canned cycle

f

Canned cycle for drilling

f

Play back

f

Mirror image double turret

f

F15 tape format

f

Graphic conversation

f

Pattern data input

f

Additional custom macro common variable

f

Macro executor

f

Multiple repetitive canned cycle 2

f

Coordinate system rotation

f

Workpiece coordinate system

f

Reader/punch control 1

f

Reader/punch control 2

f

External control of I/O device

f

368

Content      ..     11      12      13      14     ..