Content      ..     4      5      6      7     ..

FANUC Series Series 16i-TB, Series 18i-TB, Series 160i-TB, Series 180i-TB. OPERATOR’S MANUAL - page 6

B-63524EN/01

PROGRAMMING

10. TOOL FUNCTION (T FUNCTION)

Explanations

D Specification by duration

A tool life is specified either as the time of use (in minutes) or the

or number of times the

frequency of use, which depends on the parameter setting parameter No.

tool has been used

6800#2 (LTM) .

Up to 4300 minutes in time or 9999 times in frequency can be specified

for a tool life.

D Maximum number of

The number of groups to be registered and the number of tools registered

groups and tools

per group can be combined in three ways. One of the three combinations

is set by a parameter No. 6800#0, #1 (Each GS1 and GS2).

Table 10.2.1 (b) The max. number of groups and tools that can be registered

The Max. number of groups and tools

The Max. number of groups and tools

GS2

GS1

without optional function of 128 tool pairs

with optional function of 128 tool pairs

(No.6800#1)

(No.6800#0)

Number of group

Number of tool

Number of group

Number of tool

0

0

16

16

16

32

0

1

32

8

32

16

1

0

64

4

64

8

1

1

16

16

128

4

In each of the cases listed above, the maximum number of tools which can

be registered is 512 or 256 depending, respectively, on whether the option

for 128 tool life control groups is used or not. When the option is not used,

set the parameters as follows: For up to 16 groups, with up to 16 tools

in each group, set GS1 = 0 and GS2 = 0. For up to 32 groups, with up to

8 tools in each group, set GS1 = 0 and GS2 = 1. To change the

combination, change the parameter, then set program is executed with the

old tool group combination set in the NC. Whenever the parameter is

changed, be sure to reexecute the group setting program.

D A T code for registering

The same tool number may appear anywhere any times in the program of

tools

tool life data.

A T code for registering tools can usually consist of up to four digits.

When the option for 128 tool life control groups is used, however, it can

consist of up to six digits.

T ffff

ff

Tool offset number

Tool selection

When using the tool life control function, do not use tool position offset

parameters LD1 and LGN (bits 0 and 1 of parameter No. 5002).

129

10. TOOL FUNCTION (T FUNCTION)

PROGRAMMING

B-63524EN/01

Example

O0001 ;

G10L3 ;

P001L0150 ;

T0011 ;

Data of group 1

T0132 ;

T0068 ;

P002L1400 ;

T0061;

T0241 ;

Data of group 2

T0134;

T0074;

P003L0700 ;

T0012;

Data of group 3

T0202 ;

G11 ;

M02 ;

Explanations

The group numbers specified in P need not be serial. They need not be

assigned to all groups, either. When using two or more offset numbers

for the same tool in the same process, set as follows;

Tape format

Meaning

P004L0500;

The tools in group 4 are used from (1)

T0101;

to (2) to (3).

T0105;

(1)

Each tool is used 500 times (or for

T0108;

500 minutes).

T0206;

When this group is specified three

T0203;

times in one process, the offset num-

T0202;

(2)

bers are selected in the following or-

T0209;

ders:

T0304;

Tools (1): 01→05→08

T0309;

(3)

Tools (2): 06→03→02→09

P005L1200;

Tools (3): 04→09

T0405;

130

10. TOOL FUNCTION (T FUNCTION)

PROGRAMMING

B-63524EN/01

10.2.3

In machining programs, T codes are used to specify tool groups as

follows:

Specifying a Tool

Group in a Machining

Tape format

Meaning

Program

Tnn99;

Ends the tool used by now, and starts to use the tool of

the ∆∆group. “99” distinguishes this specification

from ordinary specification.

Tnn88;

Cancels the offset of the tool of the group. “88” distin-

guishes this specification from ordinary specification.

M02(M300);

Ends the machining program.

Explanations

Tape format

Meaning

T0199;

Ends the previous tool, and starts to use the tool of

the 01 group.

T0188;

Cancels the offset of the tool of the 01 group.

T0508;

Ends the tool of the 01 group. Selects tool number

05 and offset number 08.

T0500;

Cancels the offset of tool number 05.

T0299;

Ends tool number 05, and starts to use the tool of

the 02 group.

T0199;

Ends the tool of the 02 group, and starts to use the

tool of the 01 group. If more than one offset number

is specified for the tool, the second offset number is

selected. Otherwise, the previous offset number is

used.

132

B-63524EN/01

PROGRAMMING

11. AUXILIARY FUNCTION

So far, one block has been able to contain only one M code. Up to three

11.2

M codes can be specified in a single block when bit 7 (M3B) of parameter

MULTIPLE M

No. 3404 is set to 1.

COMMANDS IN A

Up to three M codes specified in a block are simultaneously output to the

SINGLE BLOCK

machine. This means that compared with the conventional method of a

single M command in a single block, a shorter cycle time can be realized

in machining.

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

Multiple M commands in a single

One M command in a single block

block

M40 ;

M40M50M60 ;

M50 ;

G28G91X0Z0 ;

M60 ;

:

G28G91X0Z0 ;

:

:

:

:

:

:

:

135

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63524EN/01

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-10 and III-9.3 for the methods

of registering and selecting programs.

138

B-63524EN/01

PROGRAMMING

12. PROGRAM CONFIGURATION

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 value following a

slash (/) at the start of a block disables the execution of some blocks (see

“optional block skip” in Section II-12.2).

139

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63524EN/01

This section describes program components other than program sections.

12.1

See Section II-12.2 for a program section.

PROGRAM

Leader section

COMPONENTS

OTHER THAN

Tape start

% TITLE ;

Program start

PROGRAM

O0001 ;

SECTIONS

(COMMENT)

Comment section

Program section

M30 ;

%

Tape end

Fig. 12.1 Program configuration

Explanations

D Tape start

The tape start indicates the start of a file that contains CNC programs.

The mark is not required when programs are entered using SYSTEM P

or ordinary personal computers. The mark is not displayed on the display

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

ISO

EIA

Name

Notation in this manual

code

code

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

ISO

EIA

Name

Notation in this manual

code

code

Program start

LF

CR

;

140

B-63524EN/01

PROGRAMMING

12. PROGRAM CONFIGURATION

NOTE

If one file contains multiple programs, the EOB code for

label skip operation must not appear before a second or

subsequent program number. However, an program start

is required at the start of a program if the preceding program

ends with %.

D Comment section

Any information enclosed by the control-out and control-in codes is

regarded as a comment and skipped by the CNC. The user can enter a

header, comments, directions to the operator, etc. There is no limit on the

length of 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

F are ignored, and thus are not read into memory. When the program in

this memory is output to an external input/output device (see Section

III-8), any comments 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 outputted 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.

141

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63524EN/01

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 CRT display

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

EIA

Notation in this

code

code

manual

Tape end

%

ER

%

142

B-63524EN/01

PROGRAMMING

12. PROGRAM CONFIGURATION

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

12.2

for program components other than program sections.

PROGRAM SECTION

CONFIGURATION

% TITLE ;

Program number

O0001 ;

N1 … ;

Sequence number

(COMMENT)

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.

When the 8-digit program number option is used, however, specify eight

digits for the program number (see Section II.12.4).

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 Section 8.4 or 10.1 in Part III.).

NOTE

Program numbers 8000 to 9999 may be used by machine

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

numbers.

143

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63524EN/01

D Sequence number and

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

block

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

code.

Table 12.2 (a) EOB code

Name

ISO

EIA

Notation in this

code

code

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 can be used to

specify whether the characters constituting comments, enclosed in “(” and

“)”, are counted when obtaining the number of characters for TV check.

The TV check function can be enabled or disabled by setting on the MDI

unit (See subsec. 11.4.7 in Part III.).

144

B-63524EN/01

PROGRAMMING

12. PROGRAM CONFIGURATION

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, V,

Coordinate axis move command

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.

Dwell

P, X, U

Dwell time

Program number

P

Subprogram number

designation

Number of

P

Number of subprogram repetitions

repetitions

Parameter

P, Q

Canned cycle parameter

NOTE

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

of a program number.

N_

G_

X_ Z_

F_

S_

T_

M_

;

Spindle

Se-

Preparatory

Dimension Feed-

Tool

Miscella-

speed

quence

function

word

function

func-

neous func-

function

number

tion

tion

Fig. 12.2 (c) 1 block (example)

145

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63524EN/01

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,

-99999.999 to

-9999.9999 to

sion

system IS-B

U, V, W,

+99999.999

+9999.9999

word

A, B, C, I,

Increment

-9999.9999 to

-999.99999 to

J, K, R,

system IS-C

+9999.9999

+999.99999

Feed

Increment

F

1 to 240000

0.01 to 9600.00

per

system IS-B

mm/min

inch/min

minute

Increment

1 to 100000

0.01 to 4000.00

system IS-C

mm/min

inch/min

Feed per revolution

F

0.0001 to

0.000001 to

500.0000

9.999999

mm/rev

inch/rev

Spindle speed function

S

0 to 20000

0 to 20000

Tool function

T

0 to 99999999

0 to 99999999

Auxiliary function

M

0 to 99999999

0 to 99999999

B

0 to 99999999

0 to 99999999

Dwell

Increment

P, X, U

0 to 99999.999s

0 to 99999.999s

system IS-B

Increment

0 to 9999.9999s

0 to 9999.9999s

system IS-C

Designation of a

P

1 to 9999

1 to 9999

program number

Number of repetitions

P

1 to 999

1 to 999

NOTE

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

of a program number.

146

B-63524EN/01

PROGRAMMING

12. PROGRAM CONFIGURATION

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 tape 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.

147

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63524EN/01

D Program end

The end of a program is indicated by punching 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 item “Optional block skip”.)

148

B-63524EN/01

PROGRAMMING

12. PROGRAM CONFIGURATION

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

12.3

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)

M98 P ffff ffff ;

↑

↑

Number of times

Subprogram

the subprogram is

number

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 9999 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.

Reference item

See Chapter 10 in Part III for the method of registering a subprogram.

149

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63524EN/01

NOTE

1

The M98 and M99 signals 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

program calls a subprogram.

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 ;

150

B-63524EN/01

PROGRAMMING

12. PROGRAM CONFIGURATION

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 … ;

N0040 … ;

Optional block skip

N0050 … ;

/

N0060 M99 P0030 ;

Optional block

OFF

N0070 … ;

skip

N0080 M02 ;

ON

D Using a subprogram only

A subprogram can be executed just like a main program by searching for

the start of the subprogram with the MDI.

(See Section 9.4 in Part III for information about search operation.)

In this case, if a block containing M99 is executed, control returns to the

start of the subprogram for repeated execution. If a block containing

M99Pn is executed, control returns to the block with sequence number n

in the subprogram for repeated execution. To terminate this program, a

block containing /M02 ; or /M30 ; must be placed at an appropriate

location, and the optional block switch must be set to off ; this switch is

to be set to on first.

N1010 … ;

N1020 … ;

N1030 … ;

N1040 M02 ;

Optional block skip

/

N1050 M99 P1020 ;

ON

151

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63524EN/01

The 8-digit program number function enables specification of program

12.4

numbers with eight digits following address O

(O00000001 to

8-DIGIT PROGRAM

O99999999).

NUMBER

Explanations

D Inhibiting editing of

Editing of subprograms O00008000 to O00008999, O00009000 to

programs

O00009999, O80000000 to O89999999, and O90000000 to O99999999

can be inhibited.

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 PQE (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

152

B-63524EN/01

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

153

12. PROGRAM CONFIGURATION

PROGRAMMING

B-63524EN/01

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-19) 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

O8-digit program number can not be used in DNC1, DNC2, ethernet,

data server, OPEN CNC, CONVERSATIONAL AUTOMATIC

PROGRAMMING FUNCTION.

154

13. FUNCTIONS TO SIMPLIFY

B-63524EN/01

PROGRAMMING

PROGRAMMING

FUNCTIONS TO SIMPLIFY PROGRAMMING

13

General

This chapter explains the following items:

13.1

CANNED CYCLE (G90, G92, G94)

13.2

MULTIPLE REPETITIVE CYCLE (G70-G76)

13.3

CANNED CYCLE FOR DRILLING (G80-G89)

13.4

CANNED GRINDING CYCLE

(FOR GRINDING MACHINE)

13.5

CHAMFERING AND CORNER R

13.6

MIRROR IMAGE FOR DOUBLE TURRET (G68, G69)

13.7

DIRECT DRAWING DIMENSIONS PROGRAMMING

13.8

RIGID TAPPING

13.9

THREE-DIMENSIONAL COORDINATE CONVERSION

(G68.1, G69.1)

NOTE

Explanatory diagrams in this chapter uses diameter

programming in X axis.

In radius programming, changes U/2 with U and X/2 with X.

155

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

There are three canned cycles : the outer diameter/internal diameter

13.1

cutting canned cycle (G90), the thread cutting canned cycle (G92), and the

CANNED CYCLE

end face turning canned cycle (G94).

(G90, G92, G94)

13.1.1

Outer Diameter /

Internal Diameter

Cutting Cycle (G90)

D Straight cutting cycle

G90X (U)__Z (W)__F__ ;

R……Rapid traverse

F……Specified by F code

X axis

Z

W

4(R)

3(F)

1(R)

U/2

2(F)

X/2

Z axis

Fig. 13.1.1 (a) Straight Cutting Cycle

In incremental programming, the sign of the numbers following address

U and W depends on the direction of paths 1 and 2. In the cycle of 14.

1 1 (a), the signs of U and W are negative.

In single block mode, operations 1, 2, 3 and 4 are performed by pressing

the cycle start button once.

156

13. FUNCTIONS TO SIMPLIFY

B-63524EN/01

PROGRAMMING

PROGRAMMING

D Taper cutting cycle

G90X(U)__ Z(W)__ R__ F__ ;

R…Rapid traverse

F…Specified by F code

X axis

4(R)

3(F)

1(R)

U/2

2(F)

R

X/2

W

Z

Z axis

Fig. 13.1.1 (b) Taper Cutting Cycle

D Signs of numbers

In incremental programming, the relationship between the signs of the

specified in the taper

numbers following address U, W, and R, and the tool paths are as follows:

cutting cycle

1. U < 0, W < 0, R < 0

2. U > 0, W < 0, R > 0

X

X

Z

Z

W

4(R)

2(F)

U/2

3(F)

1(R)

R

R

U/2

3(F)

1(R)

2(F)

W

4(R)

3. U < 0, W < 0, R > 0

4. U > 0, W < 0, R<0

U

U

at | R | x |

|

at | R | x |

|

2

2

X

X

Z

Z

W

4(R)

R

1(R)

2(F)

U/2

3(F)

U/2

3(F)

2(F)

1(R)

R

W

4(R)

157

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

13.1.2

Thread Cutting Cycle

(G92)

G92X(U)__ Z(W)__ F__ ; Lead (L) is specified.

X axis

Z

W

4(R)

3(R)

1(R)

2(F)

X/2

Z axis

R…… Rapid traverse

F…… Specified by

F code

L

(The chamfered angle in the left figure

is 45 degrees or less because of the

delay in the servo system.

Approx. 45°

r

Detailed chamfered thread

Fig. 13.1.2 (a) Straight Thread Cutting

In incremental programming, the sign of numbers following addresses U

and W depends on the direction of paths 1 and 2. That is , if the direction

of path 1 is the negative along the X axis, the value of U is negative.

The range of thread leads, limitation of spindle speed, etc. are the same

as in G32 (thread cutting). Thread chamfering can be performed in this

thread cutting cycle. A signal from the machine tool, initiates thread

chamfering. The chamfering distance is specified in a range from 0.1L

to 12.7L in 0.1L increments by parameter (No. 5130).

(In the above

expression, L is the thread lead.)

In the single block mode, operations 1, 2, 3, and 4 are performed by

pressing cycle start button once.

158

Content      ..     4      5      6      7     ..