FANUC Series 0i-MODEL F. For Lathe System OPERATOR'S MANUAL (B-64604EN-1/01)

B-64604EN-1/01

PROGRAMMING

- 89 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

Axis name and second auxiliary functions

Even if address U, V, or W is used as an axis name or second auxiliary function, data specified at address
U, V, or W in a G71 to G73 block is assumed to be that for the multiple repetitive canned cycle.

Tool nose radius compensation

When using tool nose radius compensation, specify a tool nose radius compensation command (G41,
G42) before a multiple repetitive canned cycle command (G70, G71, G72, G73) and specify the cancel
command (G40) outside the programs (from the block specified with P to the block specified with Q)
specifying a target finishing figure. If tool nose radius compensation is specified in the program
specifying a target finishing figure, alarm PS0325, “UNAVAILABLE COMMAND IS IN SHAPE
PROGRAM”, is issued.

- Multi-spindle control

When a spindle selection by address P of multi-spindle control or the command by the extended spindle
name is used, S code cannot be specified at the block of multiple repetitive canned cycle command
(G71-G73). (The alarm PS5305 “ILLEGAL SPINDLE NUMBER” is issued.)
In this case, instead of specifying S code at the block of multiple repetitive canned cycle command
(G71-G73) is specified, specify S code before the multiple repetitive canned cycle command (G71-G73)
block.

PROGRAMMING

B-64604EN-1/01

- 90 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

4.3

CANNED CYCLE FOR DRILLING

Canned cycles for drilling make it easier for the programmer to create programs. With a canned cycle, a
frequently-used machining operation can be specified in a single block with a G function; without canned
cycles, more than one block is required. In addition, the use of canned cycles can shorten the program to
save memory.
Table 4.3 (a) lists canned cycles for drilling.

Table 4.3 (a) Canned cycles for drilling

G code

Drilling axis

Hole machining

operation

Operation in the

bottom hole position

Retraction operation

Applications

G80 -

Cancel

G83 Z

axis

Cutting feed /

intermittent

Dwell

Rapid traverse

Front drilling cycle

G84

Z axis

Cutting feed

Dwell

→

spindle CCW

Cutting feed

Front tapping cycle

G85

Z axis

Cutting feed

Dwell

Cutting feed

Front boring cycle

G87 X

axis

Cutting feed /

intermittent

Dwell

Rapid traverse

Side drilling cycle

G88

X axis

Cutting feed

Dwell

→

Spindle CCW

Cutting feed

Side tapping cycle

G89

X axis

Cutting feed

Dwell

Cutting feed

Side boring cycle

NOTE

When bit 4 (NCD) of parameter No.8137 is 0, this function can be used.

Explanation

The canned cycle for drilling consists of the following six operation sequences.

Operation 1    Positioning of X (Z) and C 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 level

Operation 1

Operation 2

Point R level

Initial level

Operation 6

Operation 5

Operation 3

Operation 4

Rapid traverse

Feed

Fig. 4.3 (a) Operation sequence of canned cycle for drilling

B-64604EN-1/01

PROGRAMMING

- 91 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

Positioning axis and drilling axis

The C-axis and X- or Z-axis are used as positioning axes. The X- or Z-axis, which is not used as a
positioning axis, is used as a drilling axis. A drilling G code specifies positioning axes and a drilling axis
as shown below.
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.

Table 4.3 (b) Positioning axis and drilling axis

G code

Positioning axis

Drilling axis

G83, G84, G85

X axis, C axis

Z axis

G87, G88, G89

Z axis, C axis

X axis

G83 and G87, G84 and G88, and G85 and G89 have the same function respectively except for axes
specified as positioning axes and a drilling axis.

- Drilling mode

G83 to G85/G87 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.
The feedrate specified at F is retained also after the drilling cycle is canceled. When Q data is required, it
must be specified in each block. Once specified, the M code used for C-axis clamp/unclamp functions as
a modal code. It is canceled by specifying G80.

Return point level

In G code system A, the tool returns to the initial level from the bottom of a hole. In G code system B or
C, specifying G98 returns the tool to the initial level from the bottom of a hole and specifying G99 returns
the tool to the point R level from the bottom of a hole.
The following illustrates how the tool moves when G98 or G99 is specified (Fig. 4.3 (b)). 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

Fig. 4.3 (b)

Number of repeats

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 programming.
If it is specified in absolute programming, drilling is repeated at the same position.

Number of repeats K The maximum command value = 9999

PROGRAMMING

B-64604EN-1/01

- 92 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

When K0 is specified, drilling data is just stored without drilling being performed.

NOTE

For K, specify an integer of 0 or 1 to 9999.

M code used for C-axis clamp/unclamp

When an M code specified in parameter No. 5110 for C-axis clamp/unclamp is coded in a program, the
following operations occur.
(1) The CNC issues the M code for C-axis clamp after the tool is positioned and while the tool is being

fed in rapid traverse to the point-R level.

(2) The CNC issues the M code for C-axis unclamp (the M code for C-axis clamp +1) after the tool

retracts to the point-R level.

(3) After the CNC issues the M code for C-axis unclamp, the tool dwells for the time specified in

parameter No. 5111.

- Cancel

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

Group 01 G codes (Example)
G00 :

Positioning (rapid traverse)

G01 :

Linear interpolation

G02 :

Circular interpolation (CW)

G03 :

Circular interpolation (CCW)

Symbols in figures

Subsequent subsections explain the individual canned cycles. Figures in these explanations use the
following symbols:

Positioning (rapid traverse G00)

Cutting feed (linear interpolation G01)

Dwell specified in the program

P2 Dwell

specified

in parameter No.5111

Issuing the M code for C-axis clamp
(The value of

is specified with parameter No. 5110.)

M (

+ 1)

Issuing the M code for C-axis unclamp

B-64604EN-1/01

PROGRAMMING

- 93 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

CAUTION

1 In each canned cycle, addresses R, Z, and X are handled as follows:

: Always handled as a radius.

Z_ or X_ : Depends on diameter/radius programming.

2 For the B or C G-code system, G90 or G91 can be used to select an incremental

or absolute programming for hole position data (X, C or Z, C), the distance from
point R to the bottom of the hole (Z or X), and the distance from the initial level to
the point R level (R).

3 For canned cycles for drilling specified in the Series 10/11 format (by setting bit 1

(FCV) of parameter No. 0001 to 1 and bit 3 (F16) of parameter No. 5102 to 0),
incremental programming is used for point R data when bit 6 (RAB) of parameter
No. 5102 is set to 0.

When bit 6 (RAB) of parameter No. 5102 is set to 1, in G code system A,
absolute programming is used, and in G code system B or C, absolute or
incremental programming is used according to G90 or G91.

For canned cycles for drilling in the Series 0

-C format, incremental programming

is used for point R data.

4.3.1

Front Drilling Cycle (G83)/Side Drilling Cycle (G87)

The peck drilling cycle or high-speed peck drilling cycle is used depending on the setting in RTR, bit 2 of
parameter No. 5101. If depth of cut for each drilling is not specified, the normal drilling cycle is used.
Without using parameter RTR, the high-speed peck drilling cycle can be specified with G83.5 or G87.5
and the peck drilling cycle can be specified with G83.6 or G87.6.

High-speed peck drilling cycle (G83, G87) (bit 2 (RTR) of parameter No. 5101
=0)

This cycle performs high-speed peck drilling. The drill repeats the cycle of drilling at the cutting feedrate
and retracting the specified retraction distance intermittently to the bottom of a hole. The drill draws
cutting chips out of the hole when it retracts.

PROGRAMMING

B-64604EN-1/01

- 94 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

Format

G83 X(U)_ C(H)_ Z(W)_ R_ P_ Q_ F_ K_ M_ ;

G87 Z(W)_ C(H)_ X(U)_ R_ P_ Q_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data
Z_ or X_ :

The distance from point R to the bottom of the hole

The distance from the initial level to point R level

Dwell time at the bottom of a hole

Depth of cut for each cutting feed

F_ :

Cutting

feedrate

Number of repeats (When it is needed)

M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode)

G83 or G87 (G99 mode)

M (

+ 1), P2

Point R

Point Z

Initial level

Point R level

Point R

Point Z

M (

+ 1), P2

M code for C-axis clamp

M (

+ 1) :

M code for C-axis unclamp

P1 :

Dwell specified in the program

P2 :

Dwell specified in parameter No. 5111

Retraction distance specified in parameter No. 5114

B-64604EN-1/01

PROGRAMMING

- 95 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

Peck drilling cycle (G83, G87) (bit 2 (RTR) of parameter No. 5101 =1)

Format

G83 X(U)_ C(H)_ Z(W)_ R_ P_ Q_ F_ K_ M_ ;

G87 Z(W)_ C(H)_ X(U)_ R_ P_ Q_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data
Z_ or X_

The distance from point R to the bottom of the hole

The distance from the initial level to point R level

Dwell time at the bottom of a hole

Depth of cut for each cutting feed

F_ :

Cutting

feedrate

Number of repeats (When it is needed.)

M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode)

G83 or G87 (G99 mode)

Point R

Point Z

Initial level

M (

+ 1), P2

Point R

Point Z

Point R level

M (

+ 1), P2

M code for C-axis clamp

M (

+ 1) :

M code for C-axis unclamp

P1 :

Dwell specified in the program

P2 :

Dwell specified in parameter No. 5111

Retraction distance specified in parameter No. 5115

Example

M51 ;

Setting C-axis index mode ON

M3 S2000 ;

Rotating the drill

G00 X50.0 C0.0 ;

Positioning the drill along the X- and C-axes

G83 Z-40.0 R-5.0 Q5000 F5.0 M31 ; Drilling hole 1
C90.0 Q5000 M31 ;

Drilling hole 2

C180.0 Q5000 M31 ;

Drilling hole 3

C270.0 Q5000 M31 ;

Drilling hole 4

G80 M05 ;

Canceling the drilling cycle and stopping drill rotation

M50 ;

Setting C-axis index mode off

NOTE

If the depth of cut for each cutting feed (Q) is not commanded, normal drilling is
performed. (See the description of the drilling cycle.)

PROGRAMMING

B-64604EN-1/01

- 96 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

Drilling cycle (G83 or G87)

If depth of cut (Q) is not specified for each drilling, the normal drilling cycle is used. The tool is then
retracted from the bottom of the hole in rapid traverse.

Format

G83 X(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ;

G87 Z(W)_ C(H)_ X(U)_ R_ P_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data
Z_ or X_

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

: The distance from the initial level to point R level

: Dwell time at the bottom of a hole

F_ :

Cutting

feedrate

: Number of repeats (When it is needed.)

: M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode)

G83 or G87 (G99 mode)

Initial level

Point R

Point Z

Point R level

M (

+ 1), P2

Point R level

Point R

Point Z

M (

+ 1), P2

M code for C-axis clamp

M (

+ 1) :

M code for C-axis unclamp

P1 :

Dwell specified in the program

P2 :

Dwell specified in parameter No. 5111

Example

M51 ;

Setting C-axis index mode ON

M3 S2000 ;

Rotating the drill

G00 X50.0 C0.0 ;

Positioning the drill along the X- and C-axes

G83 Z-40.0 R-5.0 P500 F5.0 M31 ; Drilling hole 1
C90.0 M31 ;

Drilling hole 2

C180.0 M31 ;

Drilling hole 3

C270.0 M31 ;

Drilling hole 4

G80 M05 ;

Canceling the drilling cycle and stopping drill rotation

M50 ;

Setting C-axis index mode off

B-64604EN-1/01

PROGRAMMING

- 97 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

4.3.2

Front Tapping Cycle (G84) / Side Tapping Cycle (G88)

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(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ;

G88 Z(W)_ C(H)_ X(U)_ R_ P_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data
Z_ or X_

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

: The distance from the initial level to point R level

: Dwell time at the bottom of a hole

Cutting

feedrate

: Number of repeats (When it is needed.)

: M code for C-axis clamp (when it is needed.)

G84 or G88 (G98 mode)

G84 or G88 (G99 mode)

Point R

Point Z

Spindle CCW

Spindle CW

Initial level

M (

+ 1), P2

Point R

Point Z

Spindle CCW

Spindle CW

Point R level

M (

+ 1), P2

M code for C-axis clamp

M (

+ 1) :

M code for C-axis unclamp

P1 :

Dwell specified in the program

P2 :

Dwell specified in parameter No. 5111

Explanation

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.

NOTE

Bit 3 (M5T) of parameter No. 5105 specifies whether the spindle stop command
(M05) is issued before the direction in which the spindle rotates is specified with
M03 or M04. For details, refer to the operator's manual created by the machine
tool builder.

- Q command

After setting bit 6 (PCT) of parameter No. 5104 to 1, add address Q to the ordinary tapping cycle
command format and specify the depth of cut for each tapping.

PROGRAMMING

B-64604EN-1/01

- 98 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

In the peck tapping cycle, the tool is retracted to point R for each tapping. In the high-speed peck
tapping cycle, the tool is retracted by the retraction distance specified for parameter No. 5213 in advance.
Which operation is to be performed can be selected by setting bit 5 (PCP) of parameter No. 5200.

Operation

First, ordinary tapping cycle operation is explained as basic operation.

Before specifying a tapping cycle, rotate the spindle using a miscellaneous function.
1.  When a command to position the tool to a hole position, positioning is performed.
2.  When point R is specified, positioning to point R is performed.
3.  Tapping is performed to the bottom of the hole in cutting feed.
4.  When a dwell time (P) is specified, the tool dwells.
5.  Miscellaneous function M05 (spindle stop) is output and the machine enters the FIN wait state.
6.  When FIN is returned, miscellaneous function M04 (reverse spindle rotation) is output and the

machine enters the FIN wait state.

7.  When FIN is returned, the tap is removed until point R is reached in cutting feed.
8.  When a dwell time (P) is specified, the tool dwells.
9.  Miscellaneous function M05 (spindle stop) is output and the machine enters the FIN wait state.
10.  When FIN is returned, miscellaneous function M03 (forward spindle rotation) is output, and the

machine enters the FIN wait state.

11. When FIN is returned, the tool returns to the initial point in rapid traverse when return to the initial

level is specified.

When the repetitive count is specified, operation is repeated from step 1.

<1> Positioning to a hole

<2> Positioning to point R

Point R level

Hole bottom level

<3> Tapping to the bottom of the hole

<4> Dwell

<5> Output of miscellaneous function M05

<6> Output of miscellaneous function M04

<7> Return to point R

<8> Dwell

<9> Output of miscellaneous function M05

<10> Output of miscellaneous function M03

<11> Positioning to the initial point

<1> Positioning to the next hole

Workpiece

Tapping

Peck tapping cycle

When bit 6 (PCT) of parameter No. 5104 is set 1 and bit 5 (PCP) of parameter No. 5200 is set to 1, the
peck tapping cycle is used.
Step 3 of the tapping cycle operation described above changes as follows:

3-1. The tool cuts the workpiece by the depth of cut q specified by address Q.
3-2. Miscellaneous function M05 (spindle stop) is output, and the machine enters the FIN wait state.
3-3. When FIN is returned, miscellaneous function M04 (reverse spindle rotation) is output, and the

machine enters the FIN wait state.

B-64604EN-1/01

PROGRAMMING

- 99 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

3-4. When FIN is returned, the tool is retracted to point R in cutting feed.
3-5. Miscellaneous function M05 (spindle stop) is output, and the machine enters the FIN wait state.
3-6. When FIN is returned, miscellaneous function M03 (forward spindle rotation) is output, and the

machine enters the FIN wait state.

3-7. When FIN is returned, the tool moves to the position the clearance d (parameter No. 5213) apart

from the previous cutting point in cutting feed (approach).

3-1. The tool cuts the workpiece by the clearance d (parameter No. 5213) + depth of cut q (specified by

address Q).

Tapping is performed to the bottom of the hole by repeating the above steps.
When a dwell time (P) is specified, the tool dwells only when it reaches at the bottom of the hole and
reaches point R last.

Point R level

Hole bottom level

Workpiece

<2> Output of miscellaneous function M05

<3> Output of miscellaneous function M04

<5> Output of miscellaneous function M05

<6> Output of miscellaneous function M03

<1> Tapping

<4> Retraction

<7> Approach

Repeated until the bottom of the hole is reached.

q: Depth of cut

d: Clearance

<7> Approach

High-speed peck tapping cycle

When bit 6 (PCT) of parameter No. 5104 is set 1 and bit 5 (PCP) of parameter No. 5200 is set to 0, the
high-speed peck tapping cycle is used.
Step 3 of the tapping cycle operation described above changes as follows:

3-1. The tool cuts the workpiece by the depth of cut q specified by address Q.
3-2. Miscellaneous function M05 (spindle stop) is output, and the machine enters the FIN wait state.
3-3. When FIN is returned, miscellaneous function M04 (reverse spindle rotation) is output, and the

machine enters the FIN wait state.

3-4. When FIN is returned, the tool is retracted by the retraction distance d specified by parameter No.

5213 in cutting feed.

3-5. Miscellaneous function M05 (spindle stop) is output, and the machine enters the FIN wait state.
3-6. When FIN is returned, miscellaneous function M03 (forward spindle rotation) is output, and the

machine enters the FIN wait state.

PROGRAMMING

B-64604EN-1/01

- 100 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

3-1. When FIN is returned, the tool cuts the workpiece by the retraction distance d (parameter No. 5213)

+ depth of cut q (specified by address Q).

Tapping is performed to the bottom of the hole by repeating the above steps.
When a dwell time (P) is specified, the tool dwells only when it reaches at the bottom of the hole and
reaches point R.

Point R level

Hole bottom level

Workpiece

<2> Output of miscellaneous function M05

<3> Output of miscellaneous function M04

<5> Output of miscellaneous function M05

<6> Output of miscellaneous function M03

<1> Tapping

<4> Retraction

Repeated until the bottom of the hole is reached.

q: Depth of cut

d: Retraction distance

Notes

1. The depth of cut specified by address Q is stored as a modal value until the canned cycle mode is

canceled.
In both examples 1 and 2 below, address Q is not specified in the N20 block, but the peck tapping
cycle is performed because the value specified by address Q is valid as a modal value. If this
operation is not suitable, specify G80 to cancel the canned cycle mode as shown in N15 in example
3 or specify Q0 in the tapping block as shown in N20 in example 4.

Example

N10 G84 X100.0 C0.0 Z-100.0 Q20.0 ;
N20 X150.0 C90.0 ;

←

The peck tapping cycle is also performed in this block.

N30 G80 ;

Example

N10 G83 X100.0 C0.0 Z-100.0 Q20.0 ;
N20 G84 Z-100.0 ;

←

The peck tapping cycle is also performed in this block.

N30 G80 ;

Example

N10 G83 X100.0 C0.0 Z-100.0 Q20.0 ;
N15 G80 ;

←

The canned cycle mode is canceled.

N20 G84 Z-100.0 ;
N30 G80 ;

B-64604EN-1/01

PROGRAMMING

- 101 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

Example

N10 G83 X100.0 C0.0 Z-100.0 Q20.0 ;
N20 G84 Z-100.0 Q0 ;

←

Q0 is added.

N30 G80 ;

2.  The unit for the drilling axis is used as the unit of Q. Any sign is ignored.

3.  Specify a radius value at address Q even when a diameter axis is used.

4.  Perform operation in the peck tapping cycle within point R. That is, set a value which does not

exceed point R for d (parameter No. 5213).

Example

M51 ;

Setting C-axis index mode ON

M3 S2000 ;

Rotating the drill

G00 X50.0 C0.0 ;

Positioning the drill along the X- and C- axes

G84 Z-40.0 R-5.0 P500 F5.0 M31 ; Drilling hole 1
C90.0 M31 ;

Drilling hole 2

C180.0 M31 ;

Drilling hole 3

C270.0 M31 ;

Drilling hole 4

G80 M05 ;

Canceling the drilling cycle and stopping drill rotation

M50 ;

Setting C-axis index mode off

4.3.3

Front Boring Cycle (G85) / Side Boring Cycle (G89)

This cycle is used to bore a hole.

Format

G85 X(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ;

G89 Z(W)_ C(H)_ X(U)_ R_ P_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data
Z_ or X_

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

: The distance from the initial level to point R level

: Dwell time at the bottom of a hole

Cutting

feedrate

: Number of repeats (When it is needed.)

: M code for C-axis clamp (When it is needed.)

G85 or G89 (G98 mode)

G85 or G89 (G99 mode)

Point R

Point Z

Initial level

M (

+ 1), P2

Point R

Point Z

Point R level

M (

+ 1), P2

: M code for C-axis clamp

M (

+ 1) : M code for C-axis unclamp

PROGRAMMING

B-64604EN-1/01

- 102 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

: Dwell specified in the program

: Dwell specified in parameter No. 5111

Explanation

After positioning, rapid traverse is performed to point R.
Drilling is performed from point R to point Z.
After the tool reaches point Z, it returns to point R at a feedrate twice the cutting feedrate.

Example

M51 ;

Setting C-axis index mode ON

M3 S2000 ;

Rotating the drill

G00 X50.0 C0.0 ;

Positioning the drill along the X- and C-axes

G85 Z-40.0 R-5.0 P500 F5.0 M31 ; Drilling hole 1
C90.0 M31 ;

Drilling hole 2

C180.0 M31 ;

Drilling hole 3

C270.0 M31 ;

Drilling hole 4

G80 M05 ;

Canceling the drilling cycle and stopping drill rotation

M50 ;

Setting C-axis index mode off

4.3.4

Canned Cycle for Drilling Cancel (G80)

G80 cancels canned cycle for drilling.

Format

G80 ;

Explanation

Canned cycle for drilling is canceled to perform normal operation. Point R and point Z are cleared.
Other drilling data is also canceled (cleared).

Example

M51 ;

Setting C-axis index mode ON

M3 S2000 ;

Rotating the drill

G00 X50.0 C0.0 ;

Positioning the drill along the X- and C-axes.

G83 Z-40.0 R-5.0 P500 F5.0 M31 ; Drilling hole 1
C90.0 M31 ;

Drilling hole 2

C180.0 M31 ;

Drilling hole 3

C270.0 M31 ;

Drilling hole 4

G80 M05 ;

Canceling the drilling cycle and stopping drill rotation

M50 ;

Setting C-axis index mode off

4.3.5

Addition of M Code for Clamp/Unclamp in Canned Cycle for
Drilling with

Overview

Up to two pairs of M codes used for C-axis clamp/unclamp in canned cycles for drilling can be set for
each path.

Details

Set the M codes for C-axis clamp/unclamp in the following parameters.

B-64604EN-1/01

PROGRAMMING

- 103 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

Bit 4 of parameter No. 5161=1

Pair 1

Pair 2

Bit 4 of parameter No. 5161=0

M code for clamp

No.5110 No.13544

No.5110

M code for unclamp

No.13543

No.13545

(Setting in parameter No. 5110 + 1)

When the M code for clamp set in parameter No. 5110 or 13544 (valid when bit 4 (CME) of parameter
No. 5161 is set to 1) is specified in the block for a canned cycle for drilling, the specified M code is
output before the tool is fed in rapid traverse to the point-R level after positioned. The M code for
unclamp paired with that specified M code is output after the tool retracts to the point-R level.

Example 1:

When bit 4 of parameter No. 5161 is set to 1, and 68, 78, 168, and 178 are specified in parameters
Nos. 5110, 13543, 13544 and 13545, respectively, the following M codes are output.

Command Clamp Unclamp

G83X_C_...M68 M68

M78

G83X_C_...M168 M168

M178

Example 2:

When bit 4 of parameter No. 5161 is set to 0, and 68 is specified in parameter No. 5110, respectively,

the following M codes are output.

Command Clamp Unclamp

G83X_C_...M68 M68

M69

NOTE

1 Both the M codes for clamp and unclamp are set to 0, the setting of the pair is

invalid.

2 If the same M code for clamp is set for pairs 1 and 2, the setting for pair 1 that is

specified in parameter No. 13543 is used as the M code for unclamp.

4.3.6

Reducing of Waiting Time of Spindle Speed Arrival in the
Canned Cycle for Drilling

Overview

When bit 7 (SAC) of parameter No.11507 is set to 1, this function checks the spindle speed arrival signal
SAR without waiting time that is set a parameter No.3740 at starting of drilling since the second times in
canned cycle for drilling.
Also, this function is available rapid traverse to the initial lever and block overlap in rapid traverse of
positioning to a next position of hole in canned cycle for drilling. These improvements reduce the cycle
time.

Explanation

A canned cycle for drilling consists of a sequence of six operations.

Operation 1 Positioning of axes

X (Z)

and

(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

PROGRAMMING

B-64604EN-1/01

- 104 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

Operation 1

Feed

Initial level

Operation 2

Operation 6

Point R level

Operation 5

Operation 3

Rapid traverse

Operation 4

Fig. 4.3.6 (a) Operation sequence of canned cycle for drilling

When bit 7 (SAC) of parameter No.11507 is set to 0, the spindle speed arrival signal SAR is checked after
waiting for elapsing time that is set parameter No.3740 for each drilling.
When bit 7 (SAC) of parameter No.11507 is set to 1, in drilling since the second times, the spindle speed
arrival signal SAR is checked immediately that is set parameter No.3740 is not related.
However, when command and state are the following conditions, CNC is waiting for elapsing time that is
set parameter No.3740 before checking the spindle speed arrival signal SAR.

- Canned cycle for drilling is canceled by G80 or G code of group 01.
- S code is commanded.
- G code of canned cycle for drilling is commanded which is different modal G code.
- The spindle speed arrival signal SAR becomes “0”.
- CNC becomes reset state.

Applied of speed-up of each command

Table of canned cycle for drilling (Series 0

-Fformat)

G code

Function

Reducing of waiting

time for SAR

Block overlap in rapid

traverse

G83

Front drilling cycle

available

G84

Front tapping cycle
Front face rigid tapping cycle

- available

G85

Front boring cycle

available

G87

Side drilling cycle

available

G88

Side tapping cycle
Side face rigid tapping cycle

- available

G89

Side boring cycle

available

Table of canned cycle for drilling (Series 10/11 format)

G code

Function

Reducing of waiting

time for SAR

Block overlap in rapid

traverse

G81

Drilling cycle, spot drilling cycle

available

G82

Drilling cycle, counter boring available

available

G83

Peck drilling cycle

available

G83.1

High-speed peck drilling cycle

available

G84 Tapping

cycle

available

G84.2

Rigid tapping cycle

available

G85 Boring

cycle

available

G89 Boring

cycle

available

FANUC Series 0i-MODEL F. For Lathe System OPERATOR'S MANUAL (B-64604EN-1/01) - page 7