FANUC Series 0i-MC. OPERATOR’S MANUAL

B-64124EN/01

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

Sequence number

1-99999

Preparatory function

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

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

0.001-500.00

0.0001-9.9999

mm/rev

inch/rev

Spindle speed function

0-20000

Tool function

0-99999999

Auxiliary function

0-99999999

Offset number

H, D

0-400

Dwell

Increment

X, P

0-99999.999s

system IS-B

Increment

0-9999.9999s

system IS-C

Designation of a pro-

1-9999

gram number

Number of subprogram

1-999

repetitions

NOTE

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

of a program number.

133

12. PROGRAM CONFIGURATION

PROGRAMMING

B-64124EN/01

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

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

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.

134

B-64124EN/01

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”.)

135

12. PROGRAM CONFIGURATION

PROGRAMMING

B-64124EN/01

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

O0001 ;

O1000 ;

O2000 ;

O3000 ;

O4000 ;

M98P1000 ;

M98P2000 ;

M98P3000 ;

M98P4000 ;

M30 ;

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.

136

B-64124EN/01

PROGRAMMING

12. PROGRAM CONFIGURATION

NOTE

The M98 and M99 code signal and strobe signal are not

output to the machine tool.

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

N0010 0 ;

O1010 0 ;

N0020 0 ;

N1020 0 ;

N0030 M98 P21010 ;

N1030 0 ;

N0040 0 ;

N1040 0 ;

N0050 M98 P1010 ;

N1050 0 ;

N0060 0 ;

N1060 0 M99 ;

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

gram calls a subprogram.

137

12. PROGRAM CONFIGURATION

PROGRAMMING

B-64124EN/01

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 skip

N0060 M99 P0030 ;

N0070 … ;

N0080 M02 ;

138

B-64124EN/01

PROGRAMMING

12. PROGRAM CONFIGURATION

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 III-9.3 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 … ;

Optional block skip

N1040 M02 ;

N1050 M99 P1020 ;

139

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64124EN/01

FUNCTIONS TO SIMPLIFY PROGRAMMING

General

This chapter explains the following items:

13.1

CANNED CYCLE

13.2

RIGID TAPPING

13.3

CANNED GRINDING CYCLE (FOR GRINDING MACHINE)

13.4

GRINDING-WHEEL WEAR COMPENSATION BY CONTINUOUS

DRESSING (FOR GRINDING MACHINE)

13.5

IN-FEED GRINDING ALONG THE Y AND Z AXES AT THE END

OF TABLE SWING (FOR GRINDING MACHINE)

13.6

OPTIONAL ANGLE CHAMFERING AND CORNER ROUNDING

13.7

EXTERNAL MOTION FUNCTION (G81)

13.8

INDEX TABLE INDEXING FUNCTION

140

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

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

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

141

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64124EN/01

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

G18

Zp-Xp plane

G19

Yp-Zp plane

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

142

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

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. 5101 #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)

Point R

Z=0

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.

143

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64124EN/01

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)

Dwell

144

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

13.1.1

This cycle performs high-speed peck drilling. It performs intermittent

cutting feed to the bottom of a hole while removing chips from the hole.

High-speed Peck

Drilling Cycle

(G73)

Format

G73 X_ Y_ Z_ R_ Q_ F_ K_ ;

X_ Y_ : Hole position data

Z_ : The distance from point R to the bottom of the hole

R_ : The distance from the initial level to point R level

Q_ : Depth of cut for each cutting feed

F_ : Cutting feedrate

K_ : Number of repeats (if required)

G73 (G98)

G73 (G99)

Initial level

Point R level

Point R

Point Z

145

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64124EN/01

Explanations

The high-speed peck drilling cycle performs intermittent feeding along

the Z-axis. When this cycle is used, chips can be removed from the hole

easily, and a smaller value can be set for retraction. This allows, drilling

to be performed efficiently. Set the clearance, d, in parameter 5114.

The tool is retracted in rapid traverse.

Before specifying G73, rotate the spindle using a miscellaneous function

(M code).

When the G73 code and an M code are specified in the same block, the

M code is executed at the time of the first positioning operation. The

system then proceeds to the next drilling operation.

When K is used to specify the number of repeats, the M code is executed

for the first hole only; for the second and subsequent holes, the M code

is not executed.

When a tool length offset (G43, G44, or G49) is specified in the canned

cycle, the offset is applied at the time of positioning to point R.

Limitations

D Axis switching

Before the drilling axis can be changed, the canned cycle must be

canceled.

D Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is

not performed.

D Q/P

Specify Q and P in blocks that perform drilling. If they are specified in

a block that does not perform drilling, they cannot be stored as modal data.

D Cancel

Do not specify a G code of the 01 group (G00 to G03 or G60 (when the

MDL bit (bit 0 of parameter 5431) is set to 1)) and G73 in a single block.

Otherwise, G73 will be canceled.

D Tool offset

In the canned cycle mode, tool offsets are ignored.

Examples

M3 S2000 ;

Cause the spindle to start rotating.

G90 G99 G73 X300. Y-250. Z-150. R-100. Q15. F120. ;

Position, drill hole 1, then return to point R.

Y-550. ;

Position, drill hole 2, then return to point R.

Y-750. ;

Position, drill hole 3, then return to point R.

X1000. ;

Position, drill hole 4, then return to point R.

Y-550. ;

Position, drill hole 5, then return to point R.

G98 Y-750. ;

Position, drill hole 6, then return to the initial

level.

G80 G28 G91 X0 Y0 Z0 ; Return to the reference position return

M5 ;

Cause the spindle to stop rotating.

146

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

13.1.2

This cycle performs left-handed tapping. In the left-handed tapping

cycle, when the bottom of the hole has been reached, the spindle rotates

Left-handed

clockwise.

Tapping Cycle (G74)

Format

G74 X_ Y_ Z_ R_P_ F_ K_ ;

X_ Y_ : Hole position data

Z_ : The distance from point R to the bottom of the hole

R_ : The distance from the initial level to point R level

P_ : Dwell time

F_ : Cutting feedrate

K_ : Number of repeats (if required)

G74 (G98)

G74 (G99)

Initial level

Spindle

CCW

Spindle

CCW

Point R

Point R level

Point R

Point Z

Spindle CW

Explanations

Tapping is performed by turning the spindle counterclockwise. When the

bottom of the hole has been reached, the spindle is rotated clockwise for

retraction. This creates a reverse thread.

Feedrate overrides are ignored during left-handed tapping. A feed hold

does not stop the machine until the return operation is completed.

Before specifying G74, use a miscellaneous function (M code) to rotate

the spindle counterclockwise.

When the G74 command and an M code are specified in the same block,

the M code is executed at the time of the first positioning operation. The

system then proceeds to the next drilling operation.

When K is used to specify the number of repeats, the M code is executed

for the first hole only; for the second and subsequent holes, the M code

is not executed.

When a tool length offset (G43, G44, or G49) is specified in the canned

cycle, the offset is applied at the time of positioning to point R.

147

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64124EN/01

Limitations

D Axis switching

Before the drilling axis can be changed, the canned cycle must be

canceled.

D Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is

not performed.

D P

Specify P in blocks that perform drilling. If it is specified in a block that

does not perform drilling, it cannot be stored as modal data.

D Cancel

Do not specify a G code of the 01 group (G00 to G03 or G60 (when the

MDL bit (bit 0 of parameter 5431) is set to 1)) and G74 in a single block.

Otherwise, G74 will be canceled.

D Tool offset

In the canned cycle mode, tool offsets are ignored.

Examples

M4 S100 ;

Cause the spindle to start rotating.

G90 G99 G74 X300. Y-250. Z-150. R-120. F120. ;

Position, tapping hole 1, then return to point R.

Y-550. ;

Position, tapping hole 2, then return to point R.

Y-750. ;

Position, tapping hole 3, then return to point R.

X1000. ;

Position, tapping hole 4, then return to point R.

Y-550. ;

Position, tapping hole 5, then return to point R.

G98 Y-750. ;

Position, tapping hole 6, then return to the

initial level.

G80 G28 G91 X0 Y0 Z0 ; Return to the reference position return

M5 ;

Cause the spindle to stop rotating.

148

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

13.1.3

The fine boring cycle bores a hole precisely. When the bottom of the hole

has been reached, the spindle stops, and the tool is moved away from the

Fine Boring Cycle

machined surface of the workpiece and retracted.

(G76)

Format

G76 X_ Y_ Z_ R_ Q_ P_ F_ K_ ;

X_ Y_ : Hole position data

Z_ : The distance from point R to the bottom of the hole

R_ : The distance from the initial level to point R level

Q_ : Shift amount at the bottom of a hole

P_ : Dwell time at the bottom of a hole

F_ : Cutting feedrate

K_ : Number of repeats (if required)

G76 (G98)

G76 (G99)

Spindle CW

Oriented spindle stop

Initial level

Spindle CW

Tool

Point R

level

Point R

Point Z

OSS

Point Z

Shift amount q

WARNING

Q (shift at the bottom of a hole) is a modal value retained

within canned cycles. It must be specified carefully because

it is also used as the depth of cut for G73 and G83.

149

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64124EN/01

Explanations

When the bottom of the hole has been reached, the spindle is stopped at

the fixed rotation position, and the tool is moved in the direction opposite

to the tool tip and retracted. This ensures that the machined surface is not

damaged and enables precise and efficient boring to be performed.

Before specifying G76, use a miscellaneous function (M code) to rotate

the spindle.

When the G76 command and an M code are specified in the same block,

the M code is executed at the time of the first positioning operation. The

system then proceeds to the next operation.

When K is used to specify the number of repeats, the M code is executed

for the first hole only; for the second and subsequent holes, the M code

is not executed.

When a tool length offset (G43, G44, or G49) is specified in the canned

cycle, the offset is applied at the time of positioning to point R.

Limitations

D Axis switching

Before the drilling axis can be changed, the canned cycle must be

canceled.

D Boring

In a block that does not contain X, Y, Z, R, or any additional axes, boring

is not performed.

D P/Q

Be sure to specify a positive value in Q. If Q is specified with a negative

value, the sign is ignored. Set the direction of shift in bits 4 (RD1) and

5 (RD2) of parameter 5101. Specify P and Q in a block that performs

boring. If they are specified in a block that does not perform boring, they

are not stored as modal data.

D Cancel

Do not specify a G code of the 01 group (G00 to G03 or G60 (when the

MDL bit (bit 0 of parameter 5431) is set to 1)) and G76 in a single block.

Otherwise, G76 will be canceled.

D Tool offset

In the canned cycle mode, tool offsets are ignored.

Examples

M3 S500 ;

Cause the spindle to start rotating.

G90 G99 G76 X300. Y-250. Position, bore hole 1, then return to point R.

Z-150. R-120. Q5.

Orient at the bottom of the hole, then shift

by 5 mm.

P1000 F120. ;

Stop at the bottom of the hole for 1 s.

Y-550. ;

Position, drill hole 2, then return to point R.

Y-750. ;

Position, drill hole 3, then return to point R.

X1000. ;

Position, drill hole 4, then return to point R.

Y-550. ;

Position, drill hole 5, then return to point R.

G98 Y-750. ;

Position, drill hole 6, then return to the initial

level.

G80 G28 G91 X0 Y0 Z0 ; Return to the reference position return

M5 ;

Cause the spindle to stop rotating.

150

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

13.1.4

This cycle is used for normal drilling. Cutting feed is performed to the

bottom of the hole. The tool is then retracted from the bottom of the hole

Drilling Cycle, Spot

in rapid traverse.

Drilling (G81)

Format

G81 X_ Y_ Z_ R_ F_ K_ ;

X_ Y_ : Hole position data

Z_ : The distance from point R to the bottom of the hole

R_ : The distance from the initial level to point R level

F_ : Cutting feedrate

K_ : Number of repeats (if required)

G81 (G98)

G81 (G99)

Initial level

Point R level

Point R

Point Z

Explanations

After positioning along the X- and Y-axes, rapid traverse is performed

to point R.

Drilling is performed from point R to point Z.

The tool is then retracted in rapid traverse.

Before specifying G81, use a miscellaneous function (M code) to rotate

the spindle.

When the G81 command and an M code are specified in the same block,

the M code is executed at the time of the first positioning operation. The

system then proceeds to the next drilling operation.

When K is used to specify the number of repeats, the M code is performed

for the first hole only; for the second and subsequent holes, the M code

is not executed.

When a tool length offset (G43, G44, or G49) is specified in the canned

cycle, the offset is applied at the time of positioning to point R.

151

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64124EN/01

Restrictions

D Axis switching

Before the drilling axis can be changed, the canned cycle must be

canceled.

D Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is

not performed.

D Cancel

Do not specify a G code of the 01 group (G00 to G03 or G60 (when the

MDL bit (bit 0 of parameter 5431) is set to 1)) and G81 in a single block.

Otherwise, G81 will be canceled.

D Tool offset

In the canned cycle mode, tool offsets are ignored.

Examples

M3 S2000 ;

Cause the spindle to start rotating.

G90 G99 G81 X300. Y-250. Z-150. R-100. F120. ;

Position, drill hole 1, then return to point R.

Y-550. ;

Position, drill hole 2, then return to point R.

Y-750. ;

Position, drill hole 3, then return to point R.

X1000. ;

Position, drill hole 4, then return to point R.

Y-550. ;

Position, drill hole 5, then return to point R.

G98 Y-750. ;

Position, drill hole 6, then return to the initial

level.

G80 G28 G91 X0 Y0 Z0 ; Return to the reference position return

M5 ;

Cause the spindle to stop rotating.

152

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

13.1.5

This cycle is used for normal drilling.

Cutting feed is performed to the bottom of the hole. At the bottom, a dwell

Drilling Cycle Counter

is performed, then the tool is retracted in rapid traverse.

Boring Cycle

This cycle is used to drill holes more accurately with respect to depth.

(G82)

Format

G82 X_ Y_ Z_ R_ P_ F_ K_ ;

X_ Y_ : Hole position data

Z_ : The distance from point R to the bottom of the hole

R_ : The distance from the initial level to point R level

P_ : Dwell time at the bottom of a hole

F_ : Cutting feed rate

K_ : Number of repeats (if required)

G82 (G98)

G82 (G99)

Initial level

Point R level

Point R

Point Z

Explanations

After positioning along the X- and Y-axes, rapid traverse is performed

to point R.

Drilling is then performed from point R to point Z.

When the bottom of the hole has been reached, a dwell is performed. The

tool is then retracted in rapid traverse.

Before specifying G82, use a miscellaneous function (M code) to rotate

the spindle.

When the G82 command and an M code are specified in the same block,

the M code is executed at the time of the first positioning operation. The

system then proceeds to the next drilling operation.

When K is used to specify the number of repeats, the M code is executed

for the first hole only; for the second and subsequent holes, the M code

is not executed.

When a tool length offset (G43, G44, or G49) is specified in the canned

cycle, the offset is applied at the time of positioning to point R.

153

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64124EN/01

Restrictions

D Axis switching

Before the drilling axis can be changed, the canned cycle must be

canceled.

D Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is

not performed.

D P

Specify P in blocks that perform drilling. If it is specified in a block that

does not perform drilling, it cannot be stored as modal data.

D Cancel

Do not specify a G code of the 01 group (G00 to G03 or G60 (when the

MDL bit (bit 0 of parameter 5431) is set to 1)) and G83 in a single block.

Otherwise, G83 will be canceled.

D Tool offset

In the canned cycle mode, tool offsets are ignored.

Examples

M3 S2000 ;

Cause the spindle to start rotating.

G90 G99 G82 X300. Y-250. Z-150. R-100. P1000 F120. ;

Position, drill hole 2, and dwell for 1 s at the

bottom of the hole, then return to point R.

Y-550. ;

Position, drill hole 2, then return to point R.

Y-750. ;

Position, drill hole 3, then return to point R.

X1000. ;

Position, drill hole 4, then return to point R.

Y-550. ;

Position, drill hole 5, then return to point R.

G98 Y-750. ;

Position, drill hole 6, then return to the initial

level.

G80 G28 G91 X0 Y0 Z0 ; Return to the reference position return

M5 ;

Cause the spindle to stop rotating.

154

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

13.1.6

This cycle performs peck drilling.

It performs intermittent cutting feed to the bottom of a hole while

Peck Drilling Cycle

removing shavings from the hole.

(G83)

Format

G83 X_ Y_ Z_ R_ Q_ F_ K_ ;

X_ Y_ : Hole position data

Z_ : The distance from point R to the bottom of the hole

R_ : The distance from the initial level to point R level

Q_ : Depth of cut for each cutting feed

F_ : Cutting feedrate

K_ : Number of repeats (if required)

G83 (G98)

G83 (G99)

Initial level

Point R

Point R level

Point R

Point Z

Explanations

Q represents the depth of cut for each cutting feed. It must always be

specified as an incremental value.

In the second and subsequent cutting feeds, rapid traverse is performed

up to a d point just before where the last drilling ended, and cutting feed

is performed again. d is set in parameter (No.5115).

Be sure to specify a positive value in Q. Negative values are ignored.

Before specifying G83, use a miscellaneous function (M code) to rotate

the spindle.

When the G83 command and an M code are specified in the same block,

the M code is executed at the time of the first positioning operation. The

system then proceeds to the next drilling operation.

When K is used to specify the number of repeats, the M code is executed

for the first hole only; for the second and subsequent holes, the M code

is not executed.

When a tool length offset (G43, G44, or G49) is specified in the canned

cycle, the offset is applied at the time of positioning to point R.

155

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64124EN/01

Limitations

D Axis switching

Before the drilling axis can be changed, the canned cycle must be

canceled.

D Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is

not performed.

D Q

Specify Q in blocks that perform drilling. If they are specified in a block

that does not perform drilling, they cannot be stored as modal data.

D Cancel

Do not specify a G code of the 01 group (G00 to G03 or G60 (when the

MDL bit (bit 0 of parameter 5431) is set to 1)) and G83 in a single block.

Otherwise, G83 will be canceled.

D Tool offset

In the canned cycle mode, tool offsets are ignored.

Examples

M3 S2000 ;

Cause the spindle to start rotating.

G90 G99 G83 X300. Y-250. Z-150. R-100. Q15. F120. ;

Position, drill hole 1, then return to point R.

Y-550. ;

Position, drill hole 2, then return to point R.

Y-750. ;

Position, drill hole 3, then return to point R.

X1000. ;

Position, drill hole 4, then return to point R.

Y-550. ;

Position, drill hole 5, then return to point R.

G98 Y-750. ;

Position, drill hole 6, then return to the initial

level.

G80 G28 G91 X0 Y0 Z0 ; Return to the reference position return

M5 ;

Cause the spindle to stop rotating.

156

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

13.1.7

An arbor with the overload torque detection function is used to retract the

tool when the overload torque detection signal (skip signal) is detected

Small-hole peck

during drilling. Drilling is resumed after the spindle speed and cutting

drilling cycle (G83)

feedrate are changed. These steps are repeated in this peck drilling cycle.

The mode for the small-hole peck drilling cycle is selected when the M

code in parameter 5163 is specified. The cycle can be started by

specifying G83 in this mode. This mode is canceled when G80 is

specified or when a reset occurs.

Format

G83 X_ Y_ Z_ R_ Q_ F_ I_ K_ P_ ;

X_ Y_ : Hole position data

Z_ : Distance from point R to the bottom of the hole

R_ : Distance from the initial level to point R

Q_ : Depth of each cut

F_ : Cutting feedrate

I_ : Forward or backward traveling speed (same format as F above)

(If this is omitted, the values in parameters No.5172 and No.5173 are

assumed as defaults.)

K_ : Number of times the operation is repeated (if required)

P_ : Dwell time at the bottom of the hole

(If this is omitted, P0 is assumed as the default.)

G83(G98)

G83(G99)

Initial level

Point R

∆

Overload torque

∆

Point Z

Dwell

∆ : Initial clearance when the tool is retracted to point R and the clearance

from the bottom of the hole in the second or subsequent drilling

(parameter 5174)

Q : Depth of each cut

Path along which the tool travels at the rapid traverse rate

Path along which the tool travels (forward or backward) at the rapid

(

) traverse rate during the cycle specified with parameters

Path along which the tool travels at the programmed cutting feedrate

157

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64124EN/01

Explanations

D Component operations

of the cycle

*Positioning along the X-axis and Y-axis

*Positioning at point R along the Z-axis

*Drilling along the Z-axis (first drilling, depth of cut Q, incremental)

Retraction (bottom of the hole → small clearance ∆, incremental)

Retraction (bottom of the hole → point R)

Advance (point R → point at a height of clearance ∆ from the bottom of

the hole)

Drilling (second or subsequent drilling, depth of cut Q + ∆ , incremental)

*Dwell

*Return to point R (or initial level) along the Z-axis, cycle end

Acceleration/deceleration during advancing and retraction is controlled

according to the cutting feed acceleration/deceleration time constant.

When retraction is performed, the position is checked at point R.

D Specifying an M code

When the M code in parameter 5163 is specified, the system enters the

mode for the small-hole peck drilling cycle.

This M code does not wait for FIN. Care must be taken when this M code

is specified with another M code in the same block.

(Example) Mjj M03 ; → Waits for FIN.

M03 Mjj ; → Does not wait for FIN.

D Specifying a G code

When G83 is specified in the mode for the small-hole peck drilling cycle,

the cycle is started.

This continuous-state G code remains unchanged until another canned

cycle is specified or until the G code for cancelling the canned cycle is

specified. This eliminates the need for specifying drilling data in each

block when identical drilling is repeated.

D Signal indicating that the

In this cycle, the signal indicating that the small-hole peck drilling cycle

cycle is in progress

is in progress is output after the tool is positioned at the hole position

along the axes not used for drilling. Signal output continues during

positioning to point R along the drilling axis and terminates upon a return

to point R or the initial level. For details, refer to the manual of the

machine tool builder.

D Overload torque

A skip signal is used as the overload torque detection signal. The skip

detection signal

signal is effective while the tool is advancing or drilling and the tool tip

is between points R and Z. (The signal causes a retraction). For details,

refer to the manual of the machine tool builder.

158

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

D Changing the drilling

In a single G83 cycle, drilling conditions are changed for each drilling

conditions

operation (advance → drilling → retraction). Bits 1 and 2 of parameter

OLS, NOL No. 5160 can be specified to suppress the change in drilling

conditions.

Changing the cutting feedrate

The cutting feedrate programmed with the F code is changed for each

of the second and subsequent drilling operations. In parameters

No.5166 and No.5167, specify the respective rates of change applied

when the skip signal is detected and when it is not detected in the

previous drilling operation.

Cutting feedrate =F×α

<First drilling> α=1.0

<Second or subsequent drilling> α=α×βB100, where β is the rate of

change for each drilling operation

When the skip signal is detected during the previous drilling operation

:β=b1%(parameter No. 5166)

When the skip signal is not detected during the previous drilling

operation:β=b2%(parameter No. 5167)

If the rate of change in cutting feedrate becomes smaller than the rate

specified in parameter 5168, the cutting feedrate is not changed.

The cutting feedrate can be increased up to the maximum cutting

feedrate.

Changing the spindle speed

The spindle speed programmed with the S code is changed for each of

the second and subsequent advances. In parameters 5164 and 5165,

specify the rates of change applied when the skip signal is detected and

when it is not detected in the previous drilling operation.

Spindle speed =S×γ

<First drilling> γ=1.0

<Second or subsequent drilling> γ=γ×δB100, where δ is the rate of

change for each drilling operation

When the skip signal is detected during the previous drilling operation

:β=b1%(parameter No. 5164)

When the skip signal is not detected during the previous drilling

operation:β=b2%(parameter No. 5165)

When the cutting feedrate reaches the minimum rate, the spindle speed

is not changed. The spindle speed can be increased up to a value

corresponding to the maximum value of S analog data.

Advancing and retraction of the tool are not executed in the same manner

D Advance and retraction

as rapid-traverse positioning. Like cutting feed, the two operations are

carried out as interpolated operations. The speed is subjected to exponen-

tial acceleration/deceleration. Note that the tool life management func-

tion excludes advancing and retraction from the calculation of the tool

life.

159

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64124EN/01

D Specifying address I

The forward or backward traveling speed can be specified with address

I in the same format as address F, as shown below:

G83 I1000 ;

(without decimal point)

G83 I1000. ;

(with decimal point)

Both commands indicate a speed of 1000 mm/min.

Address I specified with G83 in the continuous-state mode continues to

be valid until G80 is specified or until a reset occurs.

D Functions that can be

In this canned cycle mode, the following functions can be specified:

specified

⋅ Hole position on the X-axis, Y-axis, and additional axis

⋅ Operation and branch by custom macro

⋅ Subprogram (hole position group, etc.) calling

⋅ Switching between absolute and incremental modes

⋅ Coordinate system rotation

⋅ Scaling (This command will not affect depth of cut Q or small clearance

d1.)

⋅ Dry run

⋅ Feed hold

D Single block

When single-block operation is enabled, drilling is stopped after each

retraction.

D Feedrate override

The feedrate override function works during cutting, retraction, and

advancing in the cycle.

The number of retractions made during cutting and the number of

D Custom macro interface

retractions made in response to the overload signal received during

cutting can be output to custom macro common variables (#100 to #149)

specified in parameters No.5170 and No.5171. Parameters No.5170 and

No.5171 can specify variable numbers within the range of #100 to #149.

Parameter No.5170 : Specifies the number of the common variable to

which the number of retractions made during

cutting is output.

Parameter No.5171: Specifies the number of the common variable to

which the number of retractions made in response

to the overload signal received during cutting is

output.

160

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

Examples

N01M03 S___ ;

N02Mjj ;

N03G83 X_ Y_ Z_ R_ Q_ F_ I_ K_ P_ ;

N04X_ Y_ ;

N10G80 ;

N01: Specifies forward spindle rotation and spindle speed.

N02: Specifies the M code to execute G83 as the small-hole peck drilling cycle.

The M code is specified in parameter No.5163.

N03: Specifies the small-hole peck drilling cycle. Drilling data (except K and P)

is stored and drilling is started.

N04: Drills a small, deep hole at another position with the same drilling data as

for N03.

N10: Cancels the small-hole peck drilling cycle. The M code specified in N02

is also canceled.

13.1.8

This cycle performs tapping.

In this tapping cycle, when the bottom of the hole has been reached, the

Tapping Cycle

spindle is rotated in the reverse direction.

(G84)

Format

G84 X_ Y_ Z_ R_P_ F_ K_ ;

X_ Y_ : Hole position data

Z_ : The distance from point R to the bottom of the hole

R_ : The distance from the initial level to point R level

P_ : Dwell time

F_ : Cutting feedrate

K_ : Number of repents (if required)

G84 (G98)

G84 (G99)

Initial level

Spindle CW

Point R

Point R level

Point Z

Spindle CCW

161

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64124EN/01

Explanations

Tapping is performed by rotating the spindle clockwise. When the bottom

of the hole has been reached, the spindle is rotated in the reverse direction

for retraction. This operation creates threads.

Feedrate overrides are ignored during tapping. A feed hold does not stop

the machine until the return operation is completed.

Before specifying G84, use a miscellaneous function (M code) to rotate

the spindle.

When the G84 command and an M code are specified in the same block,

the M code is executed at the time of the first positioning operation. The

system then proceeds to the next drilling operation.

When the K is used to specify number of repeats, the M code is executed

for the first hole only; for the second and subsequent holes, the M code

is not executed.

When a tool length offset (G43, G44, or G49) is specified in the canned

cycle, the offset is applied at the time of positioning to point R.

Limitations

D Axis switching

Before the drilling axis can be changed, the canned cycle must be

canceled.

D Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is

not performed.

D P

Specify P in blocks that perform drilling. If it is specified in a block that

does not perform drilling, it cannot be stored as modal data.

D Cancel

Do not specify a G code of the 01 group (G00 to G03 or G60 (when the

MDL bit (bit 0 of parameter 5431) is set to 1)) and G84 in a single block.

Otherwise, G84 will be canceled.

D Tool offset

In the canned cycle mode, tool offsets are ignored.

Examples

M3 S100 ;

Cause the spindle to start rotating.

G90 G99 G84 X300. Y-250. Z-150. R-120. P300 F120. ;

Position, drill hole 1, then return to point R.

Y-550. ;

Position, drill hole 2, then return to point R.

Y-750. ;

Position, drill hole 3, then return to point R.

X1000. ;

Position, drill hole 4, then return to point R.

Y-550. ;

Position, drill hole 5, then return to point R.

G98 Y-750. ;

Position, drill hole 6, then return to the initial

level.

G80 G28 G91 X0 Y0 Z0 ; Return to the reference position return

M5 ;

Cause the spindle to stop rotating.

162

FANUC Series 0i-MC. OPERATOR’S MANUAL - page 6