Content      ..     1      2      3      4      ..

FANUC Series 30i-MODEL B, 31i-MODEL B, 32i-MODEL B. For Machining Center System. OPERATOR'S MANUAL - page 3

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

5.1.3

Fine Boring Cycle (G76)

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 machined surface of the workpiece and retracted.

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

Initial level

Spindle orientation

Tool

Spindle CW

Point R level

Point R

Point R

P

P

OSS

Point Z

OSS

Point Z

q

q

Shift amount q

Explanation

-

Operations

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 nose and retracted. This ensures that the machined

surface is not damaged and enables precise and efficient boring to be performed.

-

Spindle rotation

Before specifying G76, use a Auxiliary function (M code) to rotate the spindle.

-

Auxiliary function

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. 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.

-

Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the

offset is applied after the time of positioning to point R.

Limitation

-

Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

- 52 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

-

Drilling

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

-

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 the parameter No.5148.

Specify P and Q in a block that performs drilling. If they are specified in a block that does not perform

drilling, they are not stored as modal data.

CAUTION

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

for drilling. It must be specified carefully because it is also used as the depth of

cut for G73 and G83.

-

Cancel

Do not specify a G code of the 01 group (G00 to G03) and G76 in a single block. Otherwise, G76 will be

canceled.

-

Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

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

M5 ;

Cause the spindle to stop rotating.

- 53 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

5.1.4

Drilling Cycle, Spot Drilling (G81)

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 in rapid traverse.

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

Point R

Point R level

Point Z

Point Z

Explanation

-

Operations

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.

-

Spindle rotation

Before specifying G81, use an auxiliary function (M code) to rotate the spindle.

-

Auxiliary function

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. 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.

-

Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the

offset is applied after the time of positioning to point R.

Limitation

-

Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

-

Drilling

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

- 54 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

-

Cancel

Do not specify a G code of the 01 group (G00 to G03) and G81 in a single block. Otherwise, G81 will be

canceled.

-

Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

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

M5 ;

Cause the spindle to stop rotating.

5.1.5

Drilling Cycle Counter Boring Cycle (G82)

This cycle is used for normal drilling.

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

retracted in rapid traverse.

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 R

Point Z

Point Z

P

P

Explanation

-

Operations

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.

- 55 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.1.6

Peck Drilling Cycle (G83)

This cycle performs peck drilling.

It performs intermittent cutting feed to the bottom of a hole while removing shavings from the hole.

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

q

q

d

d

q

q

d

d

q

q

Point Z

Point Z

Explanation

-

Operations

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.

-

Spindle rotation

Before specifying G83, use an auxiliary function (M code) to rotate the spindle.

-

Auxiliary function

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. 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.

-

Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the

offset is applied after the time of positioning to point R.

Limitation

-

Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

- 57 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.1.7

Small-Hole Peck Drilling Cycle (G83)

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

detection signal (skip signal) is detected during drilling. Drilling is resumed after the spindle speed and

cutting 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 Nos. 5172 and 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

Point R level

Point R

q

q

Δ

Δ

Δ

Overload torque

Point Z

Δ

Dwell

Overload torque

Point Z

Dwell

Δ: 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 at the programmed cutting feedrate

Path along which the tool travels at the forward or backward rate during the cycle specified with parameters

(

)

Explanations

-

Component operations of the cycle

* X- and Y-axis positioning

* Positioning at point R along the Z-axis

- 59 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

Cutting feedrate = F × α

<First drilling> α=1.0

<Second or subsequent drilling>

α=α×β÷100, 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.

2

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×δ÷100, where δ is the rate of change for each drilling operation

When the skip signal is detected during the previous drilling operation: δ=d1% (parameter No.5164)

When the skip signal is not detected during the previous drilling operation: δ=d2% (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.

-

Advance and retraction

Advancing and retraction of the tool are not executed in the same manner as rapid-traverse positioning.

Like cutting feed, the two operations are carried out as interpolated operations. Note that the tool life

management function excludes advancing and retraction from the calculation of the tool life.

-

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.

NOTE

If address I is not specified and parameter No.5172 (for backword) or No.5173 (for

forword) is set to 0, the forword or backword travel speed is same as the cutting

feedrate specified by F.

-

Functions that can be specified

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

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

• Operation and branch by custom macro

- 61 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.1.8

Tapping Cycle (G84)

This cycle performs tapping.

In this tapping cycle, when the bottom of the hole has been reached, the spindle is rotated in the reverse

direction.

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

Spindle

CW

CW

P

Point R

P

Point R

Point R level

P

Point Z

P

Point Z

Spindle CCW

Spindle CCW

Explanation

-

Operations

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.

CAUTION

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

machine until the return operation is completed.

-

Spindle rotation

Before specifying G84, use an auxiliary function (M code) to rotate the spindle.

If drilling is continuously performed with a small value specified for the distance between the hole

position and point R level or between the initial level and point R level, the normal spindle speed may not

be reached at the start of hole cutting operation. In this case, insert a dwell before each drilling operation

with G04 to delay the operation, without specifying the number of repeats for K. For some machines, the

above note may not be considered. Refer to the manual provided by the machine tool builder.

-

Auxiliary function

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. 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.

- 63 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.1.9

Boring Cycle (G85)

This cycle is used to bore a hole.

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

Point R

Point R level

Point Z

Point Z

Explanation

-

Operations

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.

-

Spindle rotation

Before specifying G85, use an auxiliary function (M code) to rotate the spindle.

-

Auxiliary function

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. 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.

-

Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the

offset is applied after the time of positioning to point R.

Limitation

-

Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

-

Drilling

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

-

Cancel

Do not specify a G code of the 01 group (G00 to G03) and G85 in a single block. Otherwise, G85 will be

canceled.

- 65 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

-

Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

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

M5 ;

Cause the spindle to stop rotating.

5.1.10 Boring Cycle (G86)

This cycle is used to bore a hole.

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

Point R level

Point Z

Point Z

Spindle stop

Spindle stop

Explanation

-

Operations

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.

-

Spindle rotation

Before specifying G86, use an auxiliary function (M code) to rotate the spindle.

If drilling is continuously performed with a small value specified for the distance between the hole

position and point R level or between the initial level and point R level, the normal spindle speed may not

be reached at the start of hole cutting operation.

- 66 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

5.1.11 Back Boring Cycle (G87)

This cycle performs accurate boring.

Format

G87 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

Q_

: Shift amount at the bottom of a hole

P_

: Dwell time at the bottom of a hole

F_

: Cutting feed rate

K_

: Number of repeats (if required)

G87 (G98)

G87 (G99)

Spindle orientation

q

Tool

OSS

Initial

level

Spindle CW

Not used

OSS

Point Z

P

Spindle CW

Shift amount q

Point R

Explanation

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 nose, positioning (rapid traverse) is performed to the bottom of

the hole (point R).

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

direction of the tool nose and the spindle is rotated clockwise to proceed to the next block operation.

-

Spindle rotation

Before specifying G87, use an auxiliary function (M code) to rotate the spindle.

If drilling is continuously performed with a small value specified for the distance between the hole

position and point R level or between the initial level and point R level, the normal spindle speed may not

be reached at the start of hole cutting operation. In this case, insert a dwell before each drilling operation

with G04 to delay the operation, without specifying the number of repeats for K. For some machines, the

above note may not be considered. Refer to the manual provided by the machine tool builder.

-

Auxiliary function

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. 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.

-

Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the

offset is applied after the time of positioning to point R.

- 68 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

5.1.12 Boring Cycle (G88)

This cycle is used to bore a hole.

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

Point R level

Point Z

Point Z

P

P

Spindle stop

Spindle stop

after dwell

after dwell

Explanation

-

Operations

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 at the bottom of the hole, then the spindle is stopped and

enters the hold state. At this time, you can switch to the manual mode and move the tool manually. Any

manual operations are available; it is desirable to finally retract the tool from the hole for safety, though.

At the restart of machining in the DNC operation or memory mode, the tool returns to the initial level or

point R level according to G98 or G99 and the spindle rotates clockwise. Then, operation is restarted

according to the programmed commands in the next block.

-

Spindle rotation

Before specifying G88, use an auxiliary function (M code) to rotate the spindle.

-

Auxiliary function

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. 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.

-

Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the

offset is applied after the time of positioning to point R.

- 70 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

5.1.13 Boring Cycle (G89)

This cycle is used to bore a hole.

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

Point R

Point R level

Point Z

Point Z

P

P

Explanation

-

Operations

This cycle is almost the same as G85. The difference is that this cycle performs a dwell at the bottom of

the hole.

-

Spindle rotation

Before specifying G89, use an auxiliary function (M code) to rotate the spindle.

-

Auxiliary function

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. 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.

-

Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the

offset is applied after the time of positioning to point R.

Limitation

-

Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

-

Drilling

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

-

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.

- 72 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

5.1.15 Example for Using Canned Cycles for Drilling

Offset value +200.0 is set in offset No.11, +190.0 is set in offset No.15, and +150.0 is set in offset No.31

Program example

;

N001

G92 X0 Y0 Z0;

Coordinate setting at reference position

N002

G90 G00 Z250.0 T11 M6;

Tool change

N003

G43 Z0 H11;

Initial level, tool length compensation

N004

S30 M3;

Spindle start

N005

G99 G81 X400.0 Y-350.0 Z-153.0 R-97.0 F120;

Positioning, then #1 drilling

N006

Y-550.0;

Positioning, then #2 drilling and point R level return

N007

G98 Y-750.0;

Positioning, then #3 drilling and initial level return

N008

G99 X1200.0;

Positioning, then #4 drilling and point R level return

N009

Y-550.0;

Positioning, then #5 drilling and point R level return

N010

G98 Y-350.0;

Positioning, then #6 drilling and initial level return

N011

G00 X0 Y0 M5;

Reference position return, spindle stop

N012

G49 Z250.0 T15 M6;

Tool length compensation cancel, tool change

N013

G43 Z0 H15;

Initial level, tool length compensation

N014

S20 M3;

Spindle start

N015

G99 G82 X550.0 Y-450.0 Z-130.0 R-97.0 P300 F70 ;

Positioning, then #7 drilling, point R level return

N016

G98 Y-650.0;

Positioning, then #8 drilling, initial level return

N017

G99 X1050.0;

Positioning, then #9 drilling, point R level return

N018

G98 Y-450.0;

Positioning, then #10 drilling, initial level return

N019

G00 X0 Y0 M5;

Reference position return, spindle stop

N020

G49 Z250.0 T31 M6;

Tool length compensation cancel, tool change

N021

G43 Z0 H31;

Initial level, tool length compensation

N022

S10 M3;

Spindle start

N023

G85 G99 X800.0 Y-350.0 Z-153.0 R47.0 F50;

Positioning, then #11 drilling, point R level return

N024

G91 Y-200.0 K2;

Positioning, then #12, 13 drilling, point R level

return

N025

G28 X0 Y0 M5;

Reference position return, spindle stop

N026

G49 Z0;

Tool length compensation cancel

N027

M0;

Program stop

- 74 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

Program using tool length offset and canned cycles

Reference position

350

#1

#11

#6

100

#7

#10

200

100

#2

#12

#5

100

#8

#9

Y

200

100

#3

#13

#4

X

400

150

250

250

150

#1 to 6

Drilling of a 10 mm diameter hole

#7 to 10

Drilling of a 20 mm diameter hole

#11 to 13

Boring of a 95 mm diameter hole (depth 50 mm)

Z

Retract position

250

Initial level

X

50

50

30

20

T 11

T 15

T 31

200

190

150

Fig. 5.1.15 (a) Example for using canned cycles for drilling

5.2

IN-POSITION CHECK SWITCHING FOR DRILLING

CANNED CYCLE

Overview

This function enables dedicated in-position widths to be used for drilling canned cycle.

Up to four different dedicated in-position widths are available, one for hole bottoms and three for other

than hole bottoms. Using a little large in-position width for operations at locations where no nigh

precision is required makes drilling canned cycle faster.

Explanation

Setting bit 4 (ICS) of parameter No. 5107 to 1 enables dedicated in-position widths to be used for drilling

canned cycle. Up to four different dedicated in-position widths are available, one for hole bottoms and

three for other than hole bottoms.

- 75 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

In conventional drilling canned cycle, the same operation is performed for both in-position checks

between cycles for locations where no very high precision is required (A in Fig. 5.1.15 (a)) and

in-position checks between cycles for hole bottoms where a high precision is required (B in Fig. 5.1.15

(a)) because the same in-position width is used for all cycles.

Using this function makes it possible to reduce the time needed to get in an in-position state (to reduce the

necessary cycle time) by setting a small in-position width for hole bottoms so as to assure a high precision

while setting a little large in-position width for other than hole bottoms.

Fig. 5.1.15 (a) Example of a peck drilling cycle (G83)

-

Parameters related to in-position widths

This function uses the following in-position widths.

In-position width for other than hole bottoms (regular) (parameter No. 5184)

In-position width for other than hole bottoms (for retraction in peck drilling cycle) (parameter No.

5185)

In-position width for other than hole bottoms (for shift in boring cycles (G76 and G87) (parameter

No. 5186)

In-position width for hole bottoms (parameter No. 5187)

-

Supported drilling canned cycle

The following table lists the drilling canned cycle for which this function is usable.

M

Table 5.1.15 (a) Drilling canned cycle for which this function is usable (machining center system)

G code

Use

G73

High-speed peck drilling cycle

G74

Left-handed tapping cycle

G76

Fine boring cycle

G81

Drilling cycle, spot drilling cycle

G82

Drilling cycle or counter boring cycle

G83

Peck drilling cycle / Small-hole peck drilling cycle

G84

Tapping cycle

- 76 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

G code

Use

G85

Boring cycle

G86

Boring cycle

G87

Back boring cycle

G88

Boring cycle

G89

Boring cycle

-

High-speed peck drilling cycle (G73)

M

Shown below are the points where a dedicated effective area (for in-position check) is applied in

high-speed peck drilling cycle.

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 (When it is needed)

G73(G98)

G73(G99)

Initial level

Point R

Point R

Point R level

Q

Q

d

d

Q

Q

d

d

Q

Q

Point Z

Point Z

d: Retraction distance specified in parameter No. 5114

In-position width for other than hole bottoms (regular)

In-position width for other than hole bottoms (for retraction in peck drilling cycle)

In-position width for hole bottoms

- 77 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

NOTE

When setting an effective area (for in-position check) enclosed in

, pay

attention to the retraction distance d (parameter No.5114). If the effective area is

too large for the retraction distance, it is likely that no retraction may be

performed.

-

Left-handed tapping cycle (G74)

M

Shown below are the points where a dedicated effective area (for in-position check) is applied in

left-handed tapping cycle.

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 (When it is needed)

G74(G98)

G74(G99)

Initial level

Spindle CCW

Spindle CCW

P

Point R

Point R

P

Point R level

Point Z

P

Point Z

P

Spindle CW

Spindle CW

In-position width for other than hole bottoms (regular)

In-position width for hole bottoms

CAUTION

When resuming the initial level, set an effective area (for in-position check)

enclosed in

, pay attention to the distance between point R and the

workpiece. If the effective area is too large for the distance between point R

and the workpiece, it is likely that the workpiece or tool may be damaged,

because a rapid traverse may occur before the tool retracts completely from the

workpiece.

NOTE

Enabling an in-position check at hole bottoms requires setting bit 6 of parameter

No. 5103 to 1.

- 78 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

-

Fine boring cycle (G76)

M

Shown below are the points where a dedicated effective area (for in-position check) is applied in fine

boring cycle.

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 (When it is needed)

G76(G98)

G76(G99)

Spindle CW

Spindle orientation

Initial level

Tool

Spindle CW

OSS

Point R

Point R

Point R level

P

P

OSS

Point Z

OSS

Point Z

Q

Q

Shift amount q

In-position width for other than hole bottoms (regular)

In-position width for other than hole bottoms (for shift in boring cycles (G76 and G87)

In-position width for hole bottoms

NOTE

Exercise care in setting an effective area (for in-position check) enclosed in .

If too large an effective area is set without dwelling, it is likely that no complete

cutting is done at the hole bottom of the workpiece.

A shortcut is taken, resulting

in an insufficient cutting.

- 79 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

-

Drilling cycle, spot drilling cycle G81)

M

Shown below are the points where a dedicated effective area (for in-position check) is applied in drilling

cycle or spot drilling cycle.

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 (When it is needed)

G81(G98)

G81(G99)

Initial level

Point R

Point R

Point R level

Point Z

Point Z

In-position width for other than hole bottoms (regular)

In-position width for hole bottoms

-

Drilling cycle counter boring cycle (G82)

M

Shown below are the points where a dedicated effective area (for in-position check) is applied in drilling

cycle counter drilling cycle.

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 feedrate

K_

: Number of repeats (When it is needed)

G82(G98)

G82(G99)

Initial level

Point R level

Point R

Point R

Point Z

Point Z

P

P

In-position width for other than hole bottoms (regular)

In-position width for hole bottoms

- 80 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

-

Peck drilling cycle (G83)

M

Shown below are the points where a dedicated effective area (for in-position check) is applied in peck

drilling cycle.

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 (When it is needed)

G83(G98)

G83(G99)

Initial level

Point R

Point R

Point R level

Q

Q

d

d

Q

Q

d

d

Q

Q

Point Z

Point Z

d

: Clearance specified in parameter No. 5115

In-position width for other than hole bottoms (regular)

In-position width for hole bottoms

- 81 -

Content      ..     1      2      3      4      ..