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

B-64604EN-1/01

PROGRAMMING

- 281 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

6.4.8

Restrictions on Multiple Repetitive Canned Cycle

Programmed commands

- Program memory

Programs using G70, G71, G72, or G73 must be stored in the program memory. The use of the mode in
which programs stored in the program memory are called for operation enables these programs to be
executed in other than the MEM mode. Programs using G74, G75, or G76 need not be stored in the
program memory.

Blocks in which data related to a multiple repetitive canned cycle is specified

The addresses P, Q, X, Z, U, W, and R should be specified correctly for each block.

In a block in which G70, G71, G72, or G73 is specified, the following functions cannot be specified:

•

Custom macro calls (simple call, modal call, and subprogram call)

Blocks in which data related to a target figure is specified

In the block which is specified by address P of a G71, G72 or G73, G00 or G01 code in group 01 should
be commanded. If it is not commanded, alarm PS0065, “G00/G01 IS NOT IN THE FIRST BLOCK OF
SHAPE PROGRAM” is generated.

In blocks with sequence numbers between those specified at P and Q in G70, G71, G72, and G73, the
following commands can be specified:

•

Dwell

(G04)

•

G00, G01, G02, and G03

When a circular interpolation command (G02, G03) is used, there must be no radius difference
between the start point and end point of the arc. If there is a radius difference, the target finishing
figure may not be recognized correctly, resulting in a cutting error such as excessive cutting.

•

Custom macro branch and repeat command

The branch destination must be between the sequence numbers specified at P and Q, however.
High-speed branch specified by bits 1 and 4 of parameter No. 6000 is invalid. No custom macro call
(simple, modal, or subprogram call) cannot be specified.

•

Direct drawing dimension programming command and chamfering and corner R command

Direct drawing dimension programming and chamfering and corner R require multiple blocks to be
specified. The block with the last sequence number specified at Q must not be an intermediate block
of these specified blocks.

When G70, G71, G72, or G73 is executed, the sequence number specified by address P and Q should not
be specified twice or more in the same program.

When #1 = 2500 is executed using a custom macro, 2500.000 is assigned to #1. In such a case, P#1 is
equivalent to P2500.

PROGRAMMING

B-64604EN-1/01

- 282 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

Relation with other functions

- Manual intervention

After manual intervention is performed with the manual absolute on command before the execution of a
multiple repetitive canned cycles (G70 to G76) or after the stop of the execution, when a cycle operation
starts, the manual intervention amount is canceled even with an incremental cycle start command. When
only the first plane axis is specified in G74 or only the second plane axis is specified in G74, however, the
manual intervention amount is canceled only along the specified axis.

Interruption type macro

Any interruption type macro program cannot be executed during execution of a multiple repetitive canned
cycle.

Program restart and tool retract and recover

These functions cannot be executed in a block in a multiple repetitive canned cycle.

Axis name and second auxiliary functions

Even if address U, V, W, or A is used as an axis name or second auxiliary function, data specified at
address U, V, W, or A in a G71 to G73 or G76 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.

Manual intervention

Cancellation

Example of G72

B-64604EN-1/01

PROGRAMMING

- 283 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

6.5

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 6.5 (a) lists canned cycles for drilling.

NOTE

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

Table 6.5 (a) Canned cycles for drilling

G code

Drilling operation

(-Z direction)

Operation in the bottom

hole position

Retraction operation

(-Z direction)

Applications

G80 ------

------

Canceling

G81

Cutting feed

------

Rapid traverse

Drilling, Spot drilling

G82

Cutting feed

Dwell

Rapid traverse

Drilling, Counter boring

G83

Cutting feed/intermittent

------

Rapid traverse

Peck drilling cycle

G83.1

Cutting feed/ intermittent

------

Rapid traverse

High-speed peck drilling cycle

G84

Cutting feed

Dwell

→

Spindle CCW

Cutting feed

Tapping

G84.2

Cutting feed

Dwell

→

Spindle CCW

Cutting feed

Rigid tapping

G85

Cutting feed

------

Cutting feed

Boring

G89

Cutting feed

Dwell

Cutting feed

Boring

Explanation

The canned cycle for drilling consists of the following six operation sequences.
Operation 1    Positioning of X and Z axis (Another axis may be targeted.)
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. 6.5 (a) Operation sequence of canned cycle for drilling

PROGRAMMING

B-64604EN-1/01

- 284 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

- Positioning plane

A positioning plane is determined by plane selection with G17, G18, and G19.
The axes other than the drilling axis are used as positioning axes.

- Drilling axis

Although canned cycles include tapping and boring cycles as well as drilling cycles, in this chapter, only
the term drilling will be used to refer to operations implemented with canned cycles.
The basic axis (X, Y, or Z) that does not exist on the positioning plane or its parallel axis is used as the
drilling axis.
The axis address of the drilling axis specified in the same block as the G codes (G81 to G89) determines
whether a basic axis or one of parallel axes is used as the drilling axis.
If the axis address of the drilling axis is not specified, the basic axis is used as the drilling axis.

Table 6.5 (b) Positioning plane and drilling axis

G code

Positioning plane

Drilling axis

G17 Xp-Yp-plane Zp

G18 Zp-Xp-plane Yp

G19 Yp-Zp-plane Xp

Xp : X axis or its parallel axis
Yp : Y axis or its parallel axis
Zp : Z axis or its parallel axis

- Example

Suppose parameter No. 1022 is set so that U, V, and W are the parallel axes of X, Y, and Z, respectively.

G17 G81    Z _ _:  Drilling axis is Z axis.
G17 G81    W _ _:  Drilling axis is W axis.
G18 G81    Y _ _:  Drilling axis is Y axis.
G18 G81    V _ _:  Drilling axis is V axis.
G19 G81    X _ _:  Drilling axis is X axis.
G19 G81    U _ _:  Drilling axis is U axis.

G17, G18, and G19 may be specified in a block in which G73 to G89 are not present.

CAUTION

Before switching between drilling axes, cancel canned cycles.

NOTE

The Z-axis can always be used as the drilling axis by setting FXY (bit 0 of
parameter No.5101). When FXY is 0, the Z-axis is always used as the drilling
axis.

Specification of point R

In the Series 0

command format, the distance from the initial level to point R is specified using an

incremental value during specification of point R.
In the Series 10/11 command format, the specification method depends on bit 6 (RAB) of parameter No.
5102. When RAB = 0, an incremental value is always used for specification. When RAB = 1 for G code
system A, an absolute value is used for specification. When RAB = 1 for G code system B, C, an absolute
value is used in G90 mode while an incremental value is used in G91 mode.

Series 10/11 command format

Series 0

command format

Bit 6 (RAB) of parameter No. 5102 = 1

RAB=0

G code system A

G code system B,C

G90 G91

Absolute

Incremental

B-64604EN-1/01

PROGRAMMING

- 285 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

- Diameter/radius programming

The diameter/radius specification of canned cycles for drilling R command in the series 10/11 command
format can be matched with the diameter/radius specification of the drilling axis by setting bit 7 (RDI) of
parameter No. 5102 to 1.

- P

In the following G codes, dwell operation differs between Series 10/11.

Operation of the Series 10/11 format
In G83, G83.1, G84, and G84.2, dwelling is performed only when address P is specified in a block.
Operation of Series 10/11
In G83 and G83.1, dwelling is not performed.
In G84 and G84.2, dwelling with address P can be performed by setting bit 1 (DWL) of parameter No.
6200. Address P is modal data.

- Q

Address Q is always specified by using an incremental value during specification of a radius.

Feedrate for G85 and G89

In G85 and G89, the feedrate from point Z to point R is double the cutting feedrate. For Series 10/11, it is
the same as the cutting feedrate.

- Drilling mode

G81 to G89 are modal G codes and remain in effect until canceled. When in effect, the current state is the
drilling mode.
Once drilling data is specified in the drilling mode, the data is retained until modified or canceled.
Specify all necessary drilling data at the beginning of canned cycles; when canned cycles are being
performed, specify data modifications only.

Return point level G98/G99

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. 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. 6.5 (b) Initial level and point R level

Number of repeats

To repeat drilling for equally-spaced holes, specify the number of repeats in L_.
L is effective only within the block where it is specified.

PROGRAMMING

B-64604EN-1/01

- 286 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

Specify the first hole position in incremental mode.
If it is specified in absolute mode, drilling is repeated at the same position.

Number of repeats L The maximum command value = 9999

When L0 is specified, drilling data is just stored without drilling being performed.

NOTE

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

C axis clamp

The M code for C axis clamp can be specified in the Series 0

command format, but it cannot be specified

in the Series 10/11 command format.

Disabling the Series 10/11 format

The Series 10/11 command format can be disabled only during a canned cycle for drilling by setting bit 3
(F16) of parameter No. 5102 to 1. However, the repetitive count must be specified by address L.

CAUTION

If bit 3 (F16) of parameter No. 5102 is set to 1, the settings of bits 6 (RAB) and 7
(RDI) of parameter No. 5102 are disabled, and operation when RAB=0 and
RDI=0 is performed.

- 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) or helical interpolation (CW)

G03 :

Circular interpolation (CCW) or helical 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)

P Dwell

B-64604EN-1/01

PROGRAMMING

- 287 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

6.5.1

High-speed Peck Drilling Cycle (G83.1)

This cycle performs high-speed peck drilling. It performs cutting feed intermittently while discharging
chips.

Format

G83.1 X_ Y_ Z_ R_ P_ Q_ F_ L_ ;

X_ Y_ : Hole position data
Z_

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

: The distance from the initial level to point R level

P_ :

Dwell

time

: Depth of cut for each cutting feed

F_ :

Cutting

feedrate

: Number of repeats (When it is needed)

G83.1 (G98 mode)

G83.1 (G99 mode)

Point R

Point Z

Initial level

Point R level

Point R

Point Z

Explanation

- Operations

Since intermittent feed in the Z-axis direction makes discharge of chips easier and allows the fine setting
of the escaping amount, efficient machining can be performed.
Escape amount d is set in parameter No. 5114.
Escaping moves in rapid traverse.

- Spindle rotation

Before specifying G83.1, use an auxiliary function (M code) to rotate the spindle.

- Auxiliary function

If the G83.1 command and an M code are specified in the same block, the M code is executed at the first
positioning. When repetitive count L is specified, the operation above is performed for the first time and
the M code is not performed second and later times.

Limitation

- Axis switching

Before switching between drilling axes, cancel canned cycles for drilling.

PROGRAMMING

B-64604EN-1/01

- 288 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

- Drilling

In a block that does not include X, Y, Z, R, or an additional axis, drilling is not performed.

- P

Dwelling is performed only when address P is specified in a block.

- Q

Q must be specified in a block in which drilling is instructed. Otherwise, data is not stored as modal data.

- Cancel

The G codes (G00 to G03) in group 01 must not be specified in the block in which G83.1 is specified.
This cancels G83.1.

6.5.2

Drilling Cycle, Spot Drilling Cycle (G81)

The normal drilling cycle is used. The tool is then retracted from the bottom of the hole in rapid traverse.

Format

G81 X_ Y_ Z_ R_ F_ L_ ;

X_ Y_ : Hole position data
Z_

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

: The distance from the initial level to point R level

F_ :

Cutting

feedrate

: Number of repeats (When it is needed.)

G81 (G98 mode)

G81 (G99 mode)

Initial level

Point R

Point Z

Point R level

Point R

Point Z

Explanation

- Operations

Rapid traverse to the point R level is performed after positioning of the X- and Y- axes.
Then, drilling is performed from point R level to point Z.
Escaping moves in rapid traverse.

- Spindle rotation

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

- Auxiliary function

If the G81 command and an M code are specified in the same block, the M code is executed at the first
positioning. When repetitive count L is specified, the operation above is performed for the first time and
the M code is not performed second and later times.

B-64604EN-1/01

PROGRAMMING

- 289 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

Limitation

- Axis switching

Before switching between drilling axes, cancel canned cycles for drilling.

- Drilling

In a block that does not include X, Y, Z, R, or an additional axis, drilling is not performed.

- Cancel

The G codes (G00 to G03) in group 01 must not be specified in the block in which G81 is specified. This
cancels G81.

6.5.3

Drilling Cycle, Counter Boring (G82)

The normal drilling cycle is used. Cutting feed is performed to the bottom of the hole, dwelling is
performed at the bottom, and then escaping from the bottom is performed in rapid traverse.
The accuracy of the hole depth is improved.

Format

G82 X_ Y_ Z_ R_ P_ F_ L_ ;

X_ Y_ : Hole position data
Z_

: 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.)

G81 (G98 mode)

G81 (G99 mode)

Initial level

Point R

Point Z

Point R level

Point R

Point Z

Explanation

- Operations

Rapid traverse to the point R level is performed after positioning of the X- and Y- axes.
Then, drilling is performed from point R level to point Z.
Dwelling is performed at the bottom of the hole and then escaping is performed in rapid traverse.

- Spindle rotation

Before specifying G82, use an auxiliary function (M code) to rotate the spindle.

- Auxiliary function

If the G82 command and an M code are specified in the same block, the M code is executed at the first
positioning. When repetitive count L is specified, the operation above is performed for the first time and
the M code is not performed second and later times.

PROGRAMMING

B-64604EN-1/01

- 290 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

Limitation

- Axis switching

Before switching between drilling axes, cancel canned cycles for drilling.

- Drilling

In a block that does not include X, Y, Z, R, or an additional axis, drilling is not performed.

- P

P must be specified in a block in which drilling is instructed. Otherwise, data is not stored as modal data.

- Cancel

The G codes (G00 to G03) in group 01 must not be specified in the block in which G82 is specified. This
cancels G82.

6.5.4

Peck Drilling Cycle (G83)

Peck drilling is performed.
Cutting feed is performed intermittently to the bottom of the hole while chips are discharged.

Format

G83 X_ Y_ Z_ R_ P_ Q_ F_ L_ ;

X_ Y_ : Hole position data
Z_

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

: The distance from the initial level to point R level

P_ :

Dwell

time

: Depth of cut for each cutting feed

F_ :

Cutting

feedrate

: Number of repeats (When it is needed.)

G83 (G98 mode)

G83 (G99 mode)

Point R

Point Z

Initial level

Point R

Point Z

Point R level

Explanation

- Operations

Q indicates the depth of cut for each operation and is specified by an incremental value.
In the second and later cutting operations, rapid traverse is changed to cutting feed at the point distance
"d" back from the previously drilled position. "d" is set in parameter No. 5115.
A positive value must be specified for Q. A negative value is ignored.

B-64604EN-1/01

PROGRAMMING

- 291 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

- Spindle rotation

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

- Auxiliary function

If the G83 command and an M code are specified in the same block, the M code is executed at the first
positioning. When repetitive count L is specified, the operation above is performed for the first time and
the M code is not performed second and later times.

Limitation

- Axis switching

Before switching between drilling axes, cancel canned cycles for drilling.

- Drilling

In a block that does not include X, Y, Z, R, or an additional axis, drilling is not performed.

- P

Dwelling is performed only when address P is specified in a block.

- Q

Q must be specified in a block in which drilling is instructed. Otherwise, data is not stored as modal data.

- Cancel

The G codes (G00 to G03) in group 01 must not be specified in the block in which G83 is specified. This
cancels G83.

PROGRAMMING

B-64604EN-1/01

- 292 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

6.5.5

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_ L_ ;

X_ Y_ : Hole position data
Z_

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

: The distance from the initial level to point R level

P_ :

Dwell

time

F_ :

Cutting

feedrate

: Number of repeats (When it is needed.)

G84 (G98 mode)

G84 (G99 mode)

Point R

Point Z

Spindle CCW

Spindle CW

Initial level

Point R

Point Z

Spindle CCW

Spindle CW

Point R level

Explanation

- Operations

Tapping is performed by rotating the spindle clockwise.

CAUTION

Feedrate override is ignored during tapping. In addition, applying feed hold does
not stop the machine until return operation is completed.

- Spindle rotation

Before specifying G84, use an auxiliary function (M code) to rotate the spindle.
When drilling in which the distance from the hole position and initial level to the point R level is short is
continuously performed, the spindle may not reach the normal speed by the time cutting operation for the
hole is ready to be performed. In this case, reserve a time by inserting dwelling by G04 before each
drilling operation without specifying repetitive count L.
Since this consideration may not be required depending on the machine type, refer to the manual issued
by the machine tool builder.

- Auxiliary function

If the G84 command and an M code are specified in the same block, the M code is executed at the first
positioning. When repetitive count L is specified, the operation above is performed for the first time and
the M code is not performed second and later times.

B-64604EN-1/01

PROGRAMMING

- 293 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

Limitation

- Axis switching

Before switching between drilling axes, cancel canned cycles for drilling.

- Drilling

In a block that does not include X, Y, Z, R, or an additional axis, drilling is not performed.

- P

Dwelling is performed only when address P is specified in a block.

- Cancel

The G codes (G00 to G03) in group 01 must not be specified in the block in which G84 is specified. This
cancels G84.

NOTE

Set M5T (bit 6 of parameter No. 5101) to specify whether the spindle stop
command (M05) is specified before the command for rotating the spindle in the
forward or reverse direction (M03 or M04) is specified.

For details, refer to the manual issued by the machine tool builder.

6.5.6

Tapping Cycle (G84.2)

Controlling the spindle motor in the same way as a servo motor executes the high-speed tapping cycle.

Format

G84.2 X(U)_ C(H)_ Z(W)_ R_ P_ F_ L_ S_ ;

X_ C_ or Z_C_ :

Hole position data

Z_ or X_ : 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

: Number of repeats (When it is needed.)

S_ :

Spindle

speed

G84.2 (G98 mode)

G84.2 (G99 mode)

Point R

Point Z

Spindle CCW

Spindle stop

Initial level

Spindle stop

Spindle CW

Spindle stop

Point R

Point Z

Spindle CCW

Spindle stop

Point R level

Spindle stop

Spindle CW

Spindle stop

PROGRAMMING

B-64604EN-1/01

- 294 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

A G code cannot discriminate between the front face tapping cycle and side face tapping cycle using
Series 10/11 format commands.    The drilling axis is determined by plane selection (G17, G18, or G19).
Specify the plane selection that becomes equivalent to the front face tapping cycle or side face tapping
cycle as appropriate.    (When bit 0 (FXY) of parameter No. 5101 is set to 0, the Z-axis is used as the
drilling axis.    When the bit is set to 1, place selection is as follows.)

Plane selection

Drilling axis

G17 Xp-Yp plane

G18 Zp-Xp plane

G19 Yp-Zp plane

Xp:  X-axis or an axis parallel to it
Yp:  Y-axis or an axis parallel to it
Zp:  Z-axis or an axis parallel to it

Explanation

- Operations

The tool is positioned along the X- and Y-axes, then moves to the point R level in rapid traverse.
Tapping is performed from the point R level to point Z, after which the spindle stops and the tool dwells.
Then, the spindle starts reverse rotation, the tool is retracted to the point R level, and the spindle stops.
After that, when G98 is specified, the tool moves to the initial level in rapid traverse.
During tapping, the feedrate override and spindle override are assumed to be 100%.  For retraction
(operation 5), however, a fixed override of up to 2000% can be applied by setting bit 4 (DOV) of
parameter No. 5200, bit 3 (OVU) of parameter No. 5201, and parameter No. 5211.

- Thread lead

In the feed per minute mode, feedrate

spindle speed = thread lead.

In the feed per rotation mode, feedrate = thread lead.

Limitation

- Axis switching

Before switching between drilling axes, cancel canned cycles for drilling. If the drilling axis is changed
in the rigid mode, alarm PS0206 is issued.

- Drilling

In a block that does not include X, Y, Z, R, or an additional axis, drilling is not performed.

- P

Dwelling is performed only when address P is specified in a block.

- Cancel

The G codes (G00 to G03) in group 01 must not be specified in the block in which G84.2 is specified.
This cancels G84.2.

- Tool offset

In the canned cycle mode, tool offsets are ignored.

B-64604EN-1/01

PROGRAMMING

- 295 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

6.5.7

Boring Cycle (G85)

This cycle is used to bore a hole.

Format

G85 X_ Y_ Z_ R_ F_ L_ ;

X_ Y_ : Hole position data
Z_

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

: The distance from the initial level to point R level

F_ :

Cutting

feedrate

: Number of repeats (When it is needed.)

G85 (G98 mode)

G85 (G99 mode)

Point R

Point Z

Initial level

Point R

Point Z

Point R level

Explanation

- Operations

Rapid traverse to the point R level is performed after positioning of the X- and Y- axes.
Then, drilling is performed from point R level to point Z.
After reaching point Z, return to point R in cutting feed.

- Spindle rotation

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

- Auxiliary function

If the G85 command and an M code are specified in the same block, the M code is executed at the first
positioning. When repetitive count L is specified, the operation above is performed for the first time and
the M code is not performed second and later times.

Limitation

- Axis switching

Before switching between drilling axes, cancel canned cycles for drilling.

- Drilling

In a block that does not include X, Y, Z, R, or an additional axis, drilling is not performed.

- Cancel

The G codes (G00 to G03) in group 01 must not be specified in the block in which G85 is specified. This
cancels G85.

PROGRAMMING

B-64604EN-1/01

- 296 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

6.5.8

Boring Cycle (G89)

This cycle is used to bore a hole.

Format

G89 X_ Y_ Z_ R_ P_ F_ L_ ;

X_ Y_ : Hole position data
Z_

: 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.)

G89 (G98 mode)

G89 (G99 mode)

Point R

Point Z

Initial level

Point R

Point Z

Point R level

Explanation

- Operations

This is the same as G85, but dwelling is performed at the bottom of the hole.

- Spindle rotation

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

- Auxiliary function

If the G89 command and an M code are specified in the same block, the M code is executed at the first
positioning. When repetitive count L is specified, the operation above is performed for the first time and
the M code is not performed second and later times.

Limitation

- Axis switching

Before switching between drilling axes, cancel canned cycles for drilling.

- Drilling

In a block that does not include X, Y, Z, R, or an additional axis, drilling is not performed.

- P

P must be specified in a block in which drilling is instructed. Otherwise, data is not stored as modal data.

- Cancel

The G codes (G00 to G03) in group 01 must not be specified in the block in which G89 is specified. This
cancels G89.

FANUC Series 0i-MODEL F. For Lathe System OPERATOR'S MANUAL (B-64604EN-1/01) - page 19