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

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

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

Point R level

Point Z

190

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

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

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 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.

191

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

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 Tapping

clockwise.

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.

192

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

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.

D Subprogram call

In the canned cycle mode, specify the subprogram call command

M98P_in an independent block.

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.

193

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

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.

194

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

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.

D Subprogram call

In the canned cycle mode, specify the subprogram call command

M98P_in an independent block.

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.

195

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

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.

196

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

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.

197

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

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 (G82)

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

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.

198

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

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 G81 in a single block.

Otherwise, G81 will be canceled.

D Tool offset

In the canned cycle mode, tool offsets are ignored.

D Subprogram call

In the canned cycle mode, specify the subprogram call command

M98P_in an independent block.

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.

199

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

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.

200

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

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 G82 in a single block.

Otherwise, G82 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.

201

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

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

202

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

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.

203

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

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.

204

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

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.

Restrictions

D Subprogram call

In the canned cycle mode, specify the subprogram call command M98P_

in an independent block.

205

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

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

206

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

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.

D Subprogram call

In the canned cycle mode, specify the subprogram call command M98P_

in an independent block.

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.

207

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

13.1.9

This cycle is used to bore a hole.

Boring Cycle

(G85)

Format

G85 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 feed rate

K_ : Number of repeats (if required)

G85 (G98)

G85 (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.

When point Z has been reached, cutting feed is performed to return to

point R.

Before specifying G85, use a miscellaneous function (M code) to rotate

the spindle.

When the G85 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.

208

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

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 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 G85 in a single block.

Otherwise, G85 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 G85 X300. Y-250. Z-150. R-120. 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.

209

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

13.1.10

This cycle is used to bore a hole.

Boring Cycle

(G86)

Format

G86 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 feed rate

K_ : Number of repeats (if required)

G86 (G98)

G86 (G99)

Spindle CW

Initial level

Spindle CW

Point R

Point R level

Point Z

Spindle stop

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.

When the spindle is stopped at the bottom of the hole, the tool is retracted

in rapid traverse.

Before specifying G86, use a miscellaneous function (M code) to rotate

the spindle.

When the G86 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.

210

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

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 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 G86 in a single block.

Otherwise, G86 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 G86 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.

211

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

13.1.11

This cycle performs accurate boring.

Back Boring Cycle

(G87)

Format

G87 X_ Y_ Z_ R_ Q_ P_ F_ K_ ;

X_ Y_ : Hole position data

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

R_ : The distance from the initial level to point R

(the bottom of the hole) level

Q_ : Tool shift amount

P_ : Dwell time

F_ : Cutting feed rate

K_ : Number of repeats (if required)

G87 (G98)

G87 (G99)

Oriented spindle stop

OSS

Tool

Spindle CW

Not used

OSS

Point Z

Spindle CW

Shift amount q

Point R

WARNING

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

canned cycles. It must be specified carefully because it is

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

212

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

Explanations

After positioning along the X- and Y-axes, the spindle is stopped at the

fixed rotation position. The tool is moved in the direction opposite to the

tool tip, positioning (rapid traverse) is performed to the bottom of the hole

(point R).

The tool is then shifted in the direction of the tool tip and the spindle is

rotated clockwise. Boring is performed in the positive direction along the

Z-axis until point Z is reached.

At point Z, the spindle is stopped at the fixed rotation position again, the

tool is shifted in the direction opposite to the tool tip, then the tool is

returned to the initial level. The tool is then shifted in the direction of the

tool tip and the spindle is rotated clockwise to proceed to the next block

operation.

Before specifying G87, use a miscellaneous function (M code) to rotate

the spindle.

When the G87 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.

Restrictions

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 No.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 G87 in a single block.

Otherwise, G87 will be canceled.

D Tool offset

In the canned cycle mode, tool offsets are ignored.

D Subprogram call

In the canned cycle mode, specify the subprogram call command M98P_

in an independent block.

Examples

M3 S500 ;

Cause the spindle to start rotating.

G90 G87 X300. Y-250.

Position, bore hole 1.

Z-120. R-150. Q5.

Orient at the initial level, then shift by 5 mm.

P1000 F120. ;

Stop at point Z for 1 s.

Y-550. ;

Position, drill hole 2.

Y-750. ;

Position, drill hole 3.

X1000. ;

Position, drill hole 4.

Y-550. ;

Position, drill hole 5.

Y-750. ;

Position, drill hole 6

G80 G28 G91 X0 Y0 Z0 ;

Return to the reference position return

M5 ;

Cause the spindle to stop rotating.

213

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

13.1.12

This cycle is used to bore a hole.

Boring Cycle

(G88)

Format

G88 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)

G88 (G98)

G88 (G99)

Spindle CW

Initial level

Spindle CW

Point R

Point R level

Point Z

Spindle stop

after dwell

Explanations

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

to point R. Boring is performed from point R to point Z. When boring

is completed, a dwell is performed, then the spindle is stopped. The tool

is manually retracted from the bottom of the hole (point Z) to point R.

At point R, the spindle is rotated clockwise, and rapid traverse is

performed to the initial level.

Before specifying G88, use a miscellaneous function (M code) to rotate

the spindle.

When the G88 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.

214

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

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 G88 in a single block.

Otherwise, G88 will be canceled.

D Tool offset

In the canned cycle mode, tool offsets are ignored.

D Subprogram call

In the canned cycle mode, specify the subprogram call command M98P_

in an independent block.

Examples

M3 S2000 ;

Cause the spindle to start rotating.

G90 G99 G88 X300. Y-250. Z-150. R-100. P1000 F120. ;

Position, drill hole 1, return to point R

then 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.

215

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

13.1.13

This cycle is used to bore a hole.

Boring Cycle

(G89)

Format

G89 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)

G89 (G98)

G89 (G99)

Initial level

Point R level

Point R

Point Z

Explanations

This cycle is almost the same as G85. The difference is that this cycle

performs a dwell at the bottom of the hole.

Before specifying G89, use a miscellaneous function (M code) to rotate

the spindle.

When the G89 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.

216

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

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 G89 in a single block.

Otherwise, G89 will be canceled.

D Tool offset

In the canned cycle mode, tool offsets are ignored.

D Subprogram call

In the canned cycle mode, specify the subprogram call command

M98P_in an independent block.

Examples

M3 S100 ;

Cause the spindle to start rotating.

G90 G99 G89 X300. Y-250. Z-150. R-120. P1000 F120. ;

Position, drill hole 1, return to point R

then 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.

217

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

13.1.14

G80 cancels canned cycles.

Canned Cycle Cancel

(G80)

Format

G80 ;

Explanations

All canned cycles are canceled to perform normal operation. Point R and

point Z are cleared. This means that R = 0 and Z = 0 in incremental mode.

Other drilling data is also canceled (cleared).

Examples

M3 S100 ;

Cause the spindle to start rotating.

G90 G99 G88 X300. Y-250. Z-150. R-120. 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,

canned cycle cancel

M5 ;

Cause the spindle to stop rotating.

218

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 8