Content      ..     5      6      7      8     ..

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 7

10. TOOL FUNCTION

B-63534EN/02

PROGRAMMING

(T FUNCTION)

10.2.4

The life of a tool is specified by a usage frequency (count) or usage time

(in minutes).

Tool Life

Explanations

D Usage count

The usage count is incremented by 1 for each tool used in a program.

In other words, the usage count is incremented by 1 only when the first

tool group number and tool change command are specified after the

CNC unit enters the automatic operation state from the reset state.

CAUTION

Even if the same tool group number is specified more than

once in a program, the usage count is only incremented by

1 and no new tools are selected.

D Usage time

When a tool change is specified (M06), tool life management is started

for the tools specified by the tool group number. In tool life

management, the time during which a tool is used in the cutting mode

is counted in four second increments., If the tool group is changed

before the incremental time of four seconds elapses, the time is not

counted. The time a tool is used for single block stop, feed hold, rapid

traverse, dwell, machine lock, and interlock is not counted.

NOTE

1

When a tool is selected from available tools, tools are

searched starting from the current tool towards the lasttool

to find a tool whose life has not expired. When thelast tool

is reached during this search, the search restartsfrom the

first tool. When it has been determined that there are no

tools whose life has not expired, the last tool is selected.

When the tool currently being used is changed by tool skip

signal, the next new tool is selected using the method

described here.

2

When tool life is counted by time, the life counting can be

overridden using the tool life count override signal. An

override from 0 to 99.9 can be applied. When 0 is specified,

time is not counted. Before the override capability can be

used, bit 2 of parameter LFV No.6801 must be set.

3

When tool life counting indicates that the life of the last tool

in a group has expired, the tool change signal is output.

When tool life is managed by time, the signal is output when

the life of the last tool in the group has expired. When tool

life is managed by usage frequency (count), the signal is

output when the CNC unit is reset or the tool life count

restart M code is specified.

161

11. AUXILIARY FUNCTION

PROGRAMMING

B-63534EN/02

In general, only one M code can be specified in a block. However, up to

11.2

three M codes can be specified at once in a block by setting bit 7 (M3B)

MULTIPLE M

of parameter No. 3404 to 1. Up to three M codes specified in a block are

COMMANDS IN A

simultaneously output to the machine. This means that compared with

the conventional method of a single M command in a single block, a

SINGLE BLOCK

shorter cycle time can be realized in machining.

Explanations

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. For detailed information about the

mechanical operation restrictions on simultaneous specification of

multiple M codes in one block, refer to the manual of each machine

tool builder.

M00, M01, M02, M30, M98, M99, or M198 must not be specified

together with another M code.

Some M codes other than M00, M01, M02, M30, M98, M99, and

M198 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. To 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

Multiple M commands

in a single block

in a single block

M40 ;

M40M50M60 ;

M50 ;

G28G91X0Y0Z0 ;

M60 ;

:

G28G91X0Y0Z0 ;

:

:

:

:

:

:

:

164

B-63534EN/02

PROGRAMMING

12. PROGRAM CONFIGURATION

PROGRAM CONFIGURATION

12

General

D Main program and

There are two program types, main program and subprogram. Normally,

subprogram

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

Subprogram

Instruction 1

Instruction 1Ȁ

Instruction 2

Instruction 2Ȁ

Follow the direction of the

subprogram

Instruction n

Instruction n+1

Return to the main program

Fig. 12 (a) Main program and Subprogram

The CNC memory can hold up to 400 main programs and subprograms

(63 as standard). A main program can be selected from the stored main

programs to operate the machine. See III-9.3 or III-10 in OPERATION

for the methods of registering and selecting programs.

167

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63534EN/02

D Program components

A program consists of the following components:

Table 12 Program components

Components

Descriptions

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

Leader section

Tape start

% TITLE

;

Program start

O0001 ;

(COMMENT)

Program section

Comment section

M30 ;

%

Tape end

Fig. 12 (b) Program configuration

D Program section

A program section consists of several blocks. A program section starts

configuration

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 Z0 ;

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 II-12.2).

168

B-63534EN/02

PROGRAMMING

12. PROGRAM CONFIGURATION

This section describes program components other than program sections.

12.1

See II-12.2 for a program section.

PROGRAM

COMPONENTS

Leader section

OTHER THAN

Tape start

% TITLE

;

Program start

PROGRAM

O0001 ;

SECTIONS

(COMMENT)

Comment section

Program section

M30 ;

%

Tape end

Fig. 12.1 (a) Program configuration

Explanations

D Tape start

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 screen.

However, if the file is output,the mark is automatically output at the start

of the file.

Table 12.1 (a) Code of a tape start

Name

ISO code

EIA code

Notation in this manual

Tape start

%

ER

%

D Leader section

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 parity check is not made. So

a leader section can contain any codes except the EOB code.

D Program start

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

EIA code

Notation in this manual

Program start

LF

CR

;

169

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63534EN/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.

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.

Table 12.1 (c) Codes of a control-in and a control-out

ISO

EIA

Notation in this

Name

Meaning

code

code

manual

Control-out

(

2-4-5

(

Start of comment section

Control-in

)

2-4-7

)

End of comment section

When a program 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

A are ignored, and thus are not read into memory.

When data in memory is output on external I/O device(See III-8), the

comment sections are also output.

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 output or displayed.

During memory operation or DNC operation, all comment sections are

ignored.

The TV check function can be used for a comment section by setting

parameter CTV (bit 1 of No. 0100).

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

1

If only a control-in code is read with no matching

control-out code, the read control-in code is ignored.

2

The EOB code cannot be used in a comment.

170

B-63534EN/02

PROGRAMMING

12. PROGRAM CONFIGURATION

D Tape end

A tape end is to be placed at the end of a file containing NC programs.

If programs are entered using the automatic programming system, the

mark need not be entered.

The mark is not displayed on the screen. However, when a file is output,

the mark is automatically output at the end of the file.

If an attempt is made to execute % when M02 or M03 is not placed at the

end of the program, the P/S alarm (No. 5010) is occurred.

Table 12.1 (d) Code of a tape end

Name

ISO code

EIA code

Notation in this manual

Tape end

%

ER

%

171

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63534EN/02

This section describes elements of a program section. See II-12.1 for

12.2

program components other than program sections.

PROGRAM SECTION

CONFIGURATION

% TITLE;

Program number

O0001 ;

N1 … ;

Sequence number

(COMMENT)

Comment section

Program section

Program end

M30 ;

%

Fig. 12.2 (a) Program configuration

D Program number

A program number consisting of address O followed by a four-digit

number is assigned to each program at the beginning registered in

memory to identify the program.

In ISO code, the colon ( : ) can be used instead of O.

When no program number is specified at the start of a program, the

sequence number (N

) at the start of the program is regarded as its

program number. If a five-digit sequence number is used, the lower four

digits are registered as a program number. If the lower four digits are all

0, the program number registered immediately before added to 1 is

registered as a program number. Note, however, that N0 cannot be used

for a program number.

If there is no program number or sequence number at the start of a

program, a program number must be specified using the MDI panel when

the program is stored in memory (See III-8.4 or III-10.1)

NOTE

Program numbers 8000 to 9999 may be used by machine

tool builders, and the user may not be able to use these

numbers.

172

B-63534EN/02

PROGRAMMING

12. PROGRAM CONFIGURATION

D Sequence number and

A program consists of several commands. One command unit is called a

block

block. One block is separated from another with an EOB of end of block

code.

Table 12.2 (a) EOB code

Name

ISO code

EIA code

Notation in this manual

End of block (EOB)

LF

CR

;

At the head of a block, a sequence number consisting of address N

followed by a number not longer than five digits (1 to 99999) can be

placed. Sequence numbers can be specified in a random order, and any

numbers can be skipped. Sequence numbers may be specified for all

blocks or only for desired blocks of the program. In general, however, it

is convenient to assign sequence numbers in ascending order in phase

with the machining steps (for example, when a new tool is used by tool

replacement, and machining proceeds to a new surface with table

indexing.)

N300 X200.0 Z300.0 ; A sequence number is underlined.

Fig. 12.2 (b) Sequence number and block (example)

NOTE

N0 must not be used for the reason of file compatibility with

other CNC systems.

Program number 0 cannot be used. So 0 must not be used

for a sequence number regarded as a program number.

D TV check (Vertical parity

A parity check is made for a block on input tape vertically. If the number

check along tape)

of characters in one block (starting with the code immediately after an

EOB and ending with the next EOB) is odd, an P/S alarm (No.002) is

output. No TV check is made only for those parts that are skipped by the

label skip function. Bit 1 (CTV) of parameter No. 0100 is used to specify

whether comments enclosed in parentheses are counted as characters

during TV check. The TV check function can be enabled or disabled by

setting on the MDI unit (See III-11.4.3.).

173

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63534EN/02

D Block configuration

A block consists of one or more words. A word consists of an address

(word and address)

followed by a number some digits long. (The plus sign (+) or minus sign

(-) may be prefixed to a number.)

Word = Address + number (Example : X-1000)

For an address, one of the letters (A to Z) is used ; an address defines the

meaning of a number that follows the address. Table 12.2 (b) indicates

the usable addresses and their meanings.

The same address may have different meanings, depending on the

preparatory function specification.

Table 12.2 (b) Major functions and addresses

Function

Address

Meaning

Program number

O (*1)

Program number

Sequence number

N

Sequence number

Preparatory function

G

Specifies a motion mode (linear, arc,

etc.)

Dimension word

X, Y, Z, U,

Coordinate axis move command

V, W, A, B,

C

I, J, K

Coordinate of the arc center

R

Arc radius

Feed function

F

Rate of feed per minute,

Rate of feed per revolution

Spindle speed function

S

Spindle speed

Tool function

T

Tool number

Auxiliary function

M

On/off control on the machine tool

B

Table indexing, etc.

Offset number

D, H

Offset number

Dwell

P, X

Dwell time

Program number

P

Subprogram number

designation

Number of

P

Number of subprogram repetitions

repetitions

Parameter

P, Q

Canned cycle parameter

NOTE

^(*1) In ISO code, the colon ( : ) can also be used as the address

of a program number.

N_

G_

X_ Y_

F_

S_

T_

M_

;

Spindle

Sequence Preparatory

Dimension Feed-

Tool

Miscellaneous

speed

number

function

word

function

function

function

function

Fig. 12.2 (c) 1 block (example)

174

B-63534EN/02

PROGRAMMING

12. PROGRAM CONFIGURATION

D Major addresses and

Major addresses and the ranges of values specified for the addresses are

ranges of command

shown below. Note that these figures represent limits on the CNC side,

values

which are totally different from limits on the machine tool side. For

example, the CNC allows a tool to traverse up to about 100 m (in

millimeter input) along the X axis.

However, an actual stroke along the X axis may be limited to 2 m for a

specific machine tool.

Similarly, the CNC may be able to control a cutting federate of up to 240

m/min, but the machine tool may not allow more than 3 m/min. When

developing a program, the user should carefully read the manuals of the

machine tool as well as this manual to be familiar with the restrictions on

programming.

Table 12.2 (c) Major addresses and ranges of command values

Function

Address

Input in mm

Input in inch

Program number

O (*1)

1-9999

1-9999

Sequence number

N

1-99999

1-99999

Preparatory function

G

0-99

0-99

Dimen-

Increment

X, Y, Z,

99999.999mm

9999.9999inch

sion

system IS-B

U, V, W,

word

A, B, C,

Increment

9999.9999mm

999.99999inch

I, J, K, R,

system IS-C

Feed

Increment

F

1-240000mm/min

0.01-9600.00

per

system IS-B

inch/min

minute

Increment

1-100000mm/min

0.01-4000.00

system IS-C

inch/min

Feed per revolution

F

0.001-500.00

0.0001-9.9999

mm/rev

inch/rev

Spindle speed function

S

0-20000

0-20000

Tool function

T

0-99999999

0-99999999

Auxiliary function

M

0-99999999

0-99999999

B

0-99999999

0-99999999

Offset number

H, D

0-400

0-400

Dwell

Increment

X, P

0-99999.999s

0-99999.999s

system IS-B

Increment

0-9999.9999s

0-9999.9999s

system IS-C

Designation of a pro-

P

1-9999

1-9999

gram number

Number of subprogram

P

1-999

1-999

repetitions

NOTE

^(*1) In ISO code, the colon ( : ) can also be used as the address

of a program number.

175

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63534EN/02

D Optional block skip

When a slash followed by a number (/n (n=1 to 9)) is specified at the head

of a block, and optional block skip switch n on the machine operator panel

is set to on, the information contained in the block for which

/n

corresponding to switch number n is specified is ignored in DNC

operation or memory operation.

When optional block skip switch n is set to off, the information contained

in the block for which /n is specified is valid. This means that the operator

can determine whether to skip the block containing /n.

Number 1 for /1 can be omitted. However, when two or more optional

block skip switches are used for one block, number 1 for /1 cannot be

omitted.

Example)

(Incorrect)

(Correct)

//3 G00X10.0;

/1/3 G00X10.0;

This function is ignored when programs are loaded into memory. Blocks

containing /n are also stored in memory, regardless of how the optional

block skip switch is set.

Programs held in memory can be output, regardless of how the optional

block skip switches are set.

Optional block skip is effective even during sequence number search

operation.

Depending on the machine tool, all optional block skip switches (1 to 9)

may not be usable. Refer to manuals of the machine tool builder to find

which switches are usable.

WARNING

1

Position of a slash

A slash (/) must be specified at the head of a block. If a slash

is placed elsewhere, the information from the slash to

immediately before the EOB code is ignored.

2 Disabling an optional block skip switch

Optional block skip operation is processed when blocks are

read from memory or tape into a buffer. Even if a switch is

set to on after blocks are read into a buffer, the blocks

already read are not ignored.

NOTE

TV and TH check

When an optional block skip switch is on. TH and TV checks

are made for the skipped portions in the same way as when

the optional block skip switch is off.

176

B-63534EN/02

PROGRAMMING

12. PROGRAM CONFIGURATION

D Program end

The end of a program is indicated by programming one of the following

codes at the end of the program:

Table 12.2 (d) Code of a program end

Code

Meaning usage

M02

For main program

M30

M99

For subprogram

If one of the program end codes is executed in program execution, the

CNC terminates the execution of the program, and the reset state is set.

When the subprogram end code is executed, control returns to the

program that called the subprogram.

WARNING

A block containing an optional block skip code such as /M02

; , /M30 ; , or /M99 ; is not regarded as the end of a program,

if the optional block skip switch on the machine operator’s

panel is set to on.

(See “Optional block skip”.)

177

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63534EN/02

12.3

If a program contains a fixed sequence or frequently repeated pattern, such

a sequence or pattern can be stored as a subprogram in memory to simplify

SUBPROGRAM

the program.

(M98, M99)

A subprogram can be called from the main program.

A called subprogram can also call another subprogram.

Format

D Subprogram

configuration

One subprogram

O jjjj ;

Subprogram number

(or the colon (:) optionally in the case of ISO)

M99 ;

Program end

M99 need not constitute a separate block as indicated below.

Example) X100.0 Y100.0 M99 ;

D Subprogram call

M98 P fff ffff ;

↑

↑

Number of times

Subprogram number

the subprogram is

called repeatedly

When no repetition data is specified, the subprogram is called just once.

Explanations

When the main program calls a subprogram, it is regarded as a one-level

subprogram call. Thus, subprogram calls can be nested up to four levels

as shown below.

Main program

Subprogram

Subprogram

Subprogram

Subprogram

O0001 ;

O1000 ;

O2000 ;

O3000 ;

O4000 ;

M98P1000 ;

M98P2000 ;

M98P3000 ;

M98P4000 ;

M30 ;

M99 ;

M99 ;

M99 ;

M99 ;

(One-level nesting)

(Two-level nesting)

(Three-level nesting)

(Four-level nesting)

A single call command can repeatedly call a subprogram up to 999 times.

For compatibility with automatic programming systems, in the first

block, Nxxxx can be used instead of a subprogram number that follows

O (or :). A sequence number after N is registered as a subprogram number.

D Reference

See III-10 for the method of registering a subprogram.

178

B-63534EN/02

PROGRAMMING

12. PROGRAM CONFIGURATION

NOTE

1

The M98 and M99 code signal and strobe signal are not

output to the machine tool.

2

If the subprogram number specified by address P cannot be

found, an alarm (No. 078) is output.

Examples

l M98 P51002 ;

This command specifies ”Call the subprogram (number 1002) five times in

succession.” A subprogram call command (M98P_) can be specified in the

same block as a move command.

l X1000.0 M98 P1200 ;

This example calls the subprogram (number 1200) after an X movement.

l Execution sequence of subprograms called from a main program

Main program

Subprogram

1

2

3

N0010 … ;

O1010 … ;

N0020 … ;

N1020 … ;

N0030 M98 P21010 ;

N1030 … ;

N0040 … ;

N1040 … ;

N0050 M98 P1010 ;

N1050 … ;

N0060 … ;

N1060 … M99 ;

A subprogram can call another subprogram in the same way as a main pro-

gram calls a subprogram.

179

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63534EN/02

Special Usage

D Specifying the sequence

If P is used to specify a sequence number when a subprogram is

number for the return

terminated, control does not return to the block after the calling block, but

destination in the main

returns to the block with the sequence number specified by P. Note,

program

however, that P is ignored if the main program is operating in a mode other

than memory operation mode.

This method consumes a much longer time than the normal return method

to return to the main program.

Main program

Subprogram

N0010 … ;

O0010 … ;

N0020 … ;

N1020 … ;

N0030 M98 P1010 ;

N1030 … ;

N0040 … ;

N1040 … ;

N0050 … ;

N1050 … ;

N0060 … ;

N1060 M99 P0060 ;

D Using M99 in the main

If M99 is executed in a main program, control returns to the start of the

program

main program. For example, M99 can be executed by placing /M99 ; at

an appropriate location of the main program and setting the optional block

skip function to off when executing the main program. When M99 is

executed, control returns to the start of the main program, then execution

is repeated starting at the head of the main program.

Execution is repeated while the optional block skip function is set to off.

If the optional block skip function is set to on, the /M99 ; block is skipped

; control is passed to the next block for continued execution.

If/M99Pn ; is specified, control returns not to the start of the main

program, but to sequence number n. In this case, a longer time is required

to return to sequence number n.

N0010 … ;

N0020 … ;

N0030 … ;

Optional block skip

N0040 … ;

OFF

N0050 … ;

/

Optional block

N0060 M99 P0030 ;

skip

N0070 … ;

ON

N0080 M02 ;

180

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63534EN/02

12.4

The 8-digit program number function enables specification of program

numbers with eight digits following address O

(O00000001 to

8-DIGIT PROGRAM

O99999999).

NUMBER

Explanations

D Disabling editing of

Editing of subprograms O00008000 to O00008999, O00009000 to

programs

O00009999, O80000000 to O89999999, and O90000000 to O99999999

can be disabled.

Parameter

Program numbers for which editing is disabled

NE8(No.3202#0)

O00008000 to O00008999

NE9(No.3202#4)

O00009000 to O00009999

PRG8E(No.3204#3)

O80000000 to O89999999

PRG9E(No.3204#4)

O90000000 to O99999999

NOTE

When a wrong password has been specified for the

password function (see III-9.9), the settings of NE9 (bit 3 of

parameter No. 3202) and PRG9E (bit 4 of parameter No.

3204) cannot be changed.

D File name

For program punch by specifying a range, files are named as follows:

When punching by specifying O00000001 and O00123456:

“O00000001-G”

When punching by specifying O12345678 and O45678900:

“O12345678-G”

When 2-path control is being applied, the file name for the first path is

suffixed with “-1” and that for the second path is suffixed with “-2.”

D Special programs

Special subprogram numbers can be changed by using bit 5 (SPR) of

parameter No. 3204.

1) Macro call using G code

Program number

Parameter used to

specify G code

When SPR = 0

When SPR = 1

No.6050

O00009010

O90009010

No.6051

O00009011

O90009011

No.6052

O00009012

O90009012

No.6053

O00009013

O90009013

No.6054

O00009014

O90009014

No.6055

O00009015

O90009015

No.6056

O00009016

O90009016

No.6057

O00009017

O90009017

No.6058

O00009018

O90009018

No.6059

O00009019

O90009019

182

B-63534EN/02

PROGRAMMING

12. PROGRAM CONFIGURATION

2) Macro call using M code

Program number

Parameter used to

specify M code

When SPR = 0

When SPR = 1

No.6080

O00009020

O90009020

No.6081

O00009021

O90009021

No.6082

O00009022

O90009022

No.6083

O00009023

O90009023

No.6084

O00009024

O90009024

No.6085

O00009025

O90009025

No.6086

O00009026

O90009026

No.6087

O00009027

O90009027

No.6088

O00009028

O90009028

No.6089

O00009029

O90009029

3) Subprogram call using M code

Program number

Parameter used to

specify M code

When SPR = 0

When SPR = 1

No.6071

O00009001

O90009001

No.6072

O00009002

O90009002

No.6073

O00009003

O90009003

No.6074

O00009004

O90009004

No.6075

O00009005

O90009005

No.6076

O00009006

O90009006

No.6077

O00009007

O90009007

No.6078

O00009008

O90009008

No.6079

O00009009

O90009009

4) Macro call using T code

Program number

Parameter used to

specify T code

When SPR = 0

When SPR = 1

TCS(No.6001#5)

O00009000

O90009000

5) Macro call using ASCII code

Program number

Parameter used to

specify ASCII code

When SPR = 0

When SPR = 1

No.6090

O00009004

O90009004

No.6091

O00009005

O90009005

183

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63534EN/02

6) Pattern data function

Program numaber

When SPR = 0

When SPR = 1

O00009500

O90009500

O00009501

O90009501

O00009502

O90009502

O00009503

O90009503

O00009504

O90009504

O00009505

O90009505

O00009506

O90009506

O00009507

O90009507

O00009508

O90009508

O00009509

O90009509

O00009510

O90009510

D External program

External input signals can be used to search for a program number. A

number search

program stored in CNC memory can be selected by externally inputting

a program number, between 1 and 99999999, to the CNC. For details,

refer to the appropriate manual supplied from the machine tool builder.

Limitations

D Subprogram call

This function disables subprogram call unless FS15 tape format (see

II-18) is used. This restriction also applies to calling a program in

external I/O devices (M198).

(Example)

M98 P12345678 ;

Subprogram number only. The repetition

count is not included.

D DNC

The eight-digit program number cannot be used in DNC1, DNC2,

Ethernet, data server, open CNC, and graphic conversation functions.

184

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63534EN/02

Canned cycles make it easier for the programmer to create programs.

13.1

With a canned cycle, a frequently-used machining operation can be

CANNED CYCLE

specified in a single block with a G function; without canned cycles,

normally more than one block is required. In addition, the use of canned

cycles can shorten the program to save memory.

Table 13.1 (a) lists canned cycles.

Table 13.1 (a) Canned cycles

Operation at the

G code

Drilling(-Z direction)

Retraction(+Z direction)

Application

bottom of a hole

G73

Intermittent feed

-

Rapid traverse

High-speed peck drilling

cycle

G74

Feed

Dwell→Spindle CW

Feed

Left-hand tapping cycle

G76

Feed

Oriented spindle

Rapid traverse

Fine boring cycle

stop

G80

-

-

-

Cancel

G81

Feed

-

Rapid traverse

Drilling cycle, spot drilling

cycle

G82

Feed

Dwell

Rapid traverse

Drilling cycle, counter boring

cycle

G83

Intermittent feed

-

Rapid traverse

Peck drilling cycle

G84

Feed

Dwell→Spindle

Feed

Tapping cycle

CCW

G85

Feed

-

Feed

Boring cycle

G86

Feed

Spindle stop

Rapid traverse

Boring cycle

G87

Feed

Spindle CW

Rapid traverse

Back boring cycle

G88

Feed

Dwell→spindle stop

Manual

Boring cycle

G89

Feed

Dwell

Feed

Boring cycle

186

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

PROGRAMMING

Explanations

A canned cycle consists of a sequence of six operations (Fig. 13.1 (a))

Operation 1 Positioning of axes X and Y

(including also another axis)

Operation 2 Rapid traverse up to point R level

Operation 3 Hole machining

Operation 4 Operation at the bottom of a hole

Operation 5

Retraction to point R level

Operation 6

Rapid traverse up to the initial point

Operation 1

Initial level

Operation 2

Operation 6

Point R level

Operation 5

Operation 3

Rapid traverse

Operation 4

Feed

Fig. 13.1 Canned cycle operation sequence

D Positioning plane

The positioning plane is determined by plane selection code G17, G18,

or G19.

The positioning axis is an axis other than the drilling axis.

D Drilling axis

Although canned cycles include tapping and boring cycles as well as

drilling cycles, in this chapter, only the term drilling will be used to refer

to operations implemented with canned cycles.

The drilling axis is a basic axis (X, Y, or Z) not used to define the

positioning plane, or any axis parallel to that basic axis.

The axis (basic axis or parallel axis) used as the drilling axis is determined

according to the axis address for the drilling axis specified in the same

block as G codes G73 to G89.

If no axis address is specified for the drilling axis, the basic axis is

assumed to be the drilling axis.

Table 13.1 (b) Positioning plane and drilling axis

G code

Positioning plane

Drilling axis

G17

Xp-Yp plane

Zp

G18

Zp-Xp plane

Yp

G19

Yp-Zp plane

Xp

Xp : X axis or an axis parallel to the X axis

Yp : Y axis or an axis parallel to the Y axis

Zp : Z axis or an axis parallel to the Z axis

187

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63534EN/02

Examples

Assume that the U, V and W axes be parallel to the X, Y, and Z axes

respectively. This condition is specified by parameter No. 1022.

G17 G81 ………Z _ _ : The Z axis is used for drilling.

G17 G81 ………W _ _ : The W axis is used for drilling.

G18 G81 ………Y _ _ : The Y axis is used for drilling.

G18 G81 ………V _ _ : The V axis is used for drilling.

G19 G81 ………X _ _ : The X axis is used for drilling.

G19 G81 ………U _ _ : The U axis is used for drilling.

G17 to G19 may be specified in a block in which any of G73 to G89 is

not specified.

WARNING

Switch the drilling axis after canceling a canned cycle.

NOTE

A parameter FXY (No. 6200 #0) can be set to the Z axis

always used as the drilling axis. When FXY=0, the Z axis

is always the drilling axis.

D Travel distance along the

The travel distance along the drilling axis varies for G90 and G91 as

drilling axis G90/G91

follows:

G90 (Absolute Command)

G91 (Incremental Command)

R

R

Point R

Point R

Z=0

Z

Point Z

Z

Point Z

D Drilling mode

G73, G74, G76, and G81 to G89 are modal G codes and remain in effect

until canceled. When in effect, the current state is the drilling mode.

Once drilling data is specified in the drilling mode, the data is retained

until modified or canceled.

Specify all necessary drilling data at the beginning of canned cycles; when

canned cycles are being performed, specify data modifications only.

188

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

PROGRAMMING

D Return point level

When the tool reaches the bottom of a hole, the tool may be returned to

G98/G99

point R or to the initial level. These operations are specified with G98 and

G99. The following illustrates how the tool moves when G98 or G99 is

specified. Generally, G99 is used for the first drilling operation and G98

is used for the last drilling operation.

The initial level does not change even when drilling is performed in the

G99 mode.

G98(Return to initial level )

G99(Return to point R level)

Initial level

Point R level

D Repeat

To repeat drilling for equally-spaced holes, specify the number of repeats

in K_.

K is effective only within the block where it is specified.

Specify the first hole position in incremental mode (G91).

If it is specified in absolute mode (G90), drilling is repeated at the same

position.

Number of repeats K The maximum command value = 9999

If K0 is specified, drilling data is stored, but drilling is not performed.

D Cancel

To cancel a canned cycle, use G80 or a group 01 G code.

Group 01 G codes

G00 : Positioning (rapid traverse)

G01 : Linear interpolation

G02 : Circular interpolation or helical interpolation (CW)

G03 : Circular interpolation or helical interpolation (CCW)

G60 : Single direction positioning (when the MDL bit (bit 0 of

parameter 5431) is set to 1)

D Symbols in figures

Subsequent sections explain the individual canned cycles. Figures in

these explanations use the following symbols:

Positioning (rapid traverse G00)

Cutting feed (linear interpolation G01)

Manual feed

OSS Oriented spindle stop

(The spindle stops at a fixed rotation position)

Shift (rapid traverse G00)

P

Dwell

189

Content      ..     5      6      7      8     ..