FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Lathe System USER’S MANUAL

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

- Peck drilling cycle (G83, G87) (parameter No. 5101#2 =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

: 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)

Mα

Initial level

Mα

M (α + 1), P2

Point R level

Point R

M (α + 1), P2

Point R

Point Z

Mα

: M code for C-axis clamp

M (α + 1) : M code for C-axis unclamp

: Dwell specified in the program

: 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.)

- 104 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

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

: 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)

Mα

Initial level

Mα

Point R level

Point R

M (α + 1), P2

Point Z

Mα

: M code for C-axis clamp

M (α + 1) : M code for C-axis unclamp

: Dwell specified in the program

: 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

- 105 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

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_ Q_ F_ K_ M_ ;

G88 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 (Bit 6 (PCT) of

parameter No. 5104 = "1")

: 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)

Mα

Initial level

Spindle CW

M (α + 1), P2

Point R

Point R level

Point Z

Spindle CCW

Mα

: M code for C-axis clamp

M (α + 1) : M code for C-axis unclamp

: Dwell specified in the program

: 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.

- 106 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

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.

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.

When a command to position the tool to a hole position,

positioning is performed.

When point R is specified, positioning to point R is performed.

Tapping is performed to the bottom of the hole in cutting feed.

When a dwell time (P) is specified, the tool dwells.

Miscellaneous function M05 (spindle stop) is output and the

machine enters the FIN wait state.

When FIN is returned, miscellaneous function M04 (reverse

spindle rotation) is output and the machine enters the FIN wait

state.

When FIN is returned, the tap is removed until point R is reached

in cutting feed.

When a dwell time (P) is specified, the tool dwells.

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

- 107 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

Tapping

<1> Positioning to a hole

<1> Positioning to the next hole

<11> Positioning to the initial point

<2> Positioning to point R

Point R level

<8> Dwell

<3> Tapping to the bottom of the hole

<9> Output of miscellaneous function M05

<10> Output of miscellaneous function M03

<7> Return to point R

<4> Dwell

Hole bottom level

<5> Output of miscellaneous function M05

Workpiece

<6> Output of miscellaneous function M04

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.

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.

- 108 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

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.

q: Depth of cut

<5> Output of miscellaneous function M05

d: Clearance

<6> Output of miscellaneous function M03

<7> Approach

Point R level

<4> Retraction

<1> Tapping

<4> Retraction

<7> Approach

<1> Tapping

<2> Output of miscellaneous function M05

<3> Output of miscellaneous function M04

Repeated until the bottom of the hole is reached.

Workpiece

Hole bottom level

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.

- 109 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

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.

q: Depth of cut

d: Retraction distance

Point R level

<1> Tapping

<5> Output of miscellaneous function M05

<6> Output of miscellaneous function M03

<4> Retraction

<1> Tapping

<4> Retraction

<1> Tapping

<2> Output of miscellaneous function M05

<3> Output of miscellaneous function M04

Repeated until the bottom of the hole is reached.

Workpiece

Hole bottom level

Notes

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 1

N10 G84 X100. Y150. Z-100. Q20. ;

N20 X150. Y200 ; ← The peck tapping cycle is also performed

in this block.

N30 G80 ;

- 110 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

Example 2

N10 G83 X100. Y150. Z-100. Q20. ;

N20 G84 Z-100. ; ← The peck tapping cycle is also performed in

this block.

N30 G80 ;

Example 3

N10 G83 X100. Y150. Z-100. Q20. ;

N15 G80 ; ← The canned cycle mode is canceled.

N20 G84 Z-100. ;

N30 G80 ;

Example 4

N10 G83 X100. Y150. Z-100. Q20. ;

N20 G84 Z-100. Q0 ; ←Q0 is added.

N30 G80 ;

The unit for the reference axis that is set by parameter No. 1031,

not the unit for the drilling axis is used as the unit of Q. Any

sign is ignored.

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

used.

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

- 111 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

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)

Mα Initial level

Mα

Point R level

M (α + 1), P2

Point R

Point Z

Mα

: M code for C-axis clamp

M (α + 1) : M code for C-axis unclamp

: 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

- 112 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

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

- 113 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

4.3.5

Precautions to be Taken by Operator

- Reset and emergency stop

Even when the controller is stopped by resetting or emergency stop in

the course of drilling cycle, the drilling mode and drilling data are

saved; with this mind, therefore, restart operation.

- Single block

When drilling cycle is performed with a single block, the operation

stops at the end points of operations 1, 2, 6 in Fig. 4.3 (a).

Consequently, it follows that operation is started up 3 times to drill

one hole. The operation stops at the end points of operations 1, 2 with

the feed hold lamp ON. If there is a remaining repetitive count at the

end of operation 6, the operation is stopped by feed hold. If there is no

remaining repetitive count, the operation is stopped in the single block

stop state.

- Feed hold

When "Feed Hold" is applied between operations 3 and 5 by G84/G88,

the feed hold lamp lights up immediately if the feed hold is applied

again to operation 6.

- Override

During operation with G84 and G88, the feedrate override is 100%.

- 114 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

4.4

RIGID TAPPING

Front face tapping cycles (G84) and side face tapping cycles (G88)

can be performed either in conventional mode or rigid mode.

In conventional mode, the spindle is rotated or stopped, in

synchronization with the motion along the tapping axis according to

miscellaneous functions M03 (spindle CW rotation), M04 (spindle

CCW rotation), and M05 (spindle stop).

In rigid mode, the spindle motor is controlled in the same way as a

control motor, by the application of compensation to both motion

along the tapping axis and that of the spindle.

For rigid tapping, each turn of the spindle corresponds to a certain

amount of feed (screw lead) along the spindle axis. This also applies

to acceleration/deceleration. This means that rigid tapping does not

demand the use of float tappers as in the case of conventional tapping,

thus enabling high-speed, high-precision tapping.

When multispindle control is enabled (bit 3 (MSP) of parameter No.

8133 is set to 1), the second spindle can be used for rigid tapping.

- 115 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

4.4.1

FRONT FACE RIGID TAPPING CYCLE (G84) / SIDE FACE

RIGID TAPPING CYCLE (G88)

Controlling the spindle motor in the same way as a servo motor in

rigid mode enables high-speed tapping.

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

G84 or G88 (G98 mode)

G84 or G88 (G99 mode)

Spindle stop

Initial level

Operation 1

Operation 6

Spindle stop

Operation 2

Spindle stop

Spindle CW

Point R

Point R level

Point R

Point R level

Operation 3

Operation 5

Point Z

Spindle stop

Spindle

Spindle stop

Spindle CCW

Operation 4

P2 performs dwelling of C-axis unclamp. (The dwell time is set in

parameter No. 5111.)

In front face rigid tapping (G84), the plane first axis is used as the

drilling axis and the other axes are used as positioning axes.

Parameter RTX(No.5209#0)

Plane selection

Drilling axis

G17 Xp-Yp plane

G18 Zp-Xp plane

G19 Yp-Zp plane

1 (Note)

Xp: X axis or its parallel axis

Yp: Y axis or its parallel axis

Zp: Z axis or its parallel axis

- 116 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

NOTE

Invalid with the Series 10/11 format.

In side face rigid tapping (G88), the plane first axis is used as the

drilling axis and the other axes are used as positioning axes.

Parameter RTX(No.5209#0)

Plane selection

Drilling axis

G17 Xp-Yp plane

G18 Zp-Xp plane

G19 Yp-Zp plane

1 (Note)

Xp: X axis or its parallel axis

Yp: Y axis or its parallel axis

Zp: Z axis or its parallel axis

NOTE

Invalid with the Series 10/11 format.

(Series 10/11 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

: 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.)

: Spindle speed

C-axis clamp cannot be performed during specification of the Series 15 format.

G84.2 (G98 mode)

G84.2 (G99 mode)

Spindle stop

Initial level

Operation 1

Operation 6

Operation 2

Spindle stop

Spindle CW

Point R

Point R level

Point R

Point R level

Operation 3

Operation 5

Point Z

Spindle

Spindle CCW

Spindle stop

Operation 4

- 117 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

A G code cannot discriminate between 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/G19). Specify

the plane selection that becomes equivalent to front face tapping cycle

or side face tapping cycle as appropriate.

(When FXY (bit 0 of

parameter No. 5101) is 0, the Z-axis is used as the drilling axis. When

FXY is 1, plane selection is as follows.)

Plane selection

Drilling axis

G17 Xp-Yp plane

G18 Zp-Xp plane

G19 Yp-Zp plane

Xp: X axis or its parallel axis

Yp: Y axis or its parallel axis

Zp: Z axis or its parallel axis

Explanation

Once positioning for the X-axis (G84) or Z-axis (G88) has been

completed, the spindle is moved, by rapid traverse, to point R.

Tapping is performed from point R to point Z, after which the spindle

stops and observes a dwell time. Then, the spindle starts reverse

rotation, retracts to point R, stops rotating, then moves to the initial

level by 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 parameters DOV

(No. 5200#4), OVU (No.5201#3), and No. 5211.

- Rigid mode

Rigid mode can be specified by applying any of the following

methods:

•

Specifying M29S***** before a tapping block

•

Specifying M29S***** within a tapping block

•

Handling G84 or G88 as a G code for rigid tapping

(Set

parameter G84 (No. 5200#0) to 1.)

- Thread lead

In feed per minute mode, the feedrate divided by the spindle speed is

equal to the thread lead. In feed per rotation mode, the feedrate is

equal to the thread lead.

- Series 10/11 format command

When bit 1 (FCV) of parameter No. 0001 is set to 1, rigid tapping can

be executed with G84.2. The same operation as with G84 is

performed. The command format for the repetitive count is L,

however.

- Acceleration/deceleration after interpolation

Linear or bell-shaped acceleration/deceleration can be applied.

Details are given later.

- 118 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

- Look-ahead acceleration/deceleration before interpolation

Look-ahead acceleration/deceleration before interpolation is invalid.

- Override

Various types of override functions are invalid. The following

override functions can be enabled by setting corresponding

parameters:

• Extraction override

• Override signal

- Dry run

Dry run can be executed also in G84 (G88). When dry run is executed

at the feedrate for the drilling axis in G84 (G88), tapping is performed

according to the feedrate. Note that the spindle speed becomes faster

at a higher dry run feedrate.

- Machine lock

Machine lock can be executed also in G84 (G88).

When G84 (G88) is executed in the machine lock state, the tool does

not move along the drilling axis. Therefore, the spindle does not also

rotate.

- Reset

When a reset is performed during rigid tapping, the rigid tapping

mode is canceled and the spindle motor enters the normal mode. Note

that the G84 (G88) mode is not canceled in this case when bit 6 (CLR)

of parameter No. 3402 is set.

- Interlock

Interlock can also be applied in G84 (G88).

- Feed hold and single block

When parameter FHD (No. 5200#6) is set to 0, feed hold and single

block are invalid in the G84 (G88) mode. When this bit is set to 1,

they are valid.

- Manual feed

For rigid tapping by manual handle feed, see the section "Rigid

Tapping by Manual Handle."

With other manual operations, rigid tapping cannot be performed.

- Backlash compensation

In the rigid tapping mode, backlash compensation is applied to

compensate the lost motion when the spindle rotates clockwise or

counterclockwise. Set the amount of backlash in parameters Nos. 5321

to 5324.

Along the drilling axis, backlash compensation has been applied.

- 119 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

- C-axis clamp, C-axis unclamp

It is possible to specify an M code for mechanically fixing or releasing

the C-axis during rigid tapping. Adding an M code for clamp to the

G84 (G88) block outputs both M codes. Descriptions of timing are

provided later.

An M code for clamp is set in parameter No. 5110. An M code for

unclamp is assumed as follows depending on the setting of parameter

No. 5110.

Parameter No.5110

Non-0

The setting of parameter No.5110 +

No M codes are output.

1 is assumed.

Limitation

- Axis switching

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

canceled. If the drilling axis is changed in rigid mode, alarm PS0206

is issued.

- S commands

When a value exceeding the maximum rotation speed for the gear

being used is specified, alarm PS0200 is issued. If such a command

that the number of pulses of 8 msec is 32768 or more on the detection

unit level or the number of pulses of 8 msec is 32768 or more for a

serial spindle is specified, alarm PS0202 is issued.

For a built-in motor equipped with a detector having a resolution

of 4095 pulses per rotation, the maximum spindle speed during

rigid tapping is as follows (in the case of 8 msec):

(4095×1000÷8×60)÷4095=7500 (min^-1)

For a serial spindle

(32767×1000÷8×60)÷4095=60012(min^-1) [Note:Ideal value]

When rigid tapping is canceled, the S value used for rigid tapping is

cleared (as if S0 is specified).

- F commands

Specifying a value larger than the upper limit for cutting feed will

cause alarm PS0201 to be issued.

- Unit of F command

Metric input

Inch input

Remarks

Decimal point programming

G98

1mm/min

0.01inch/min

allowed

Decimal point programming

G99

0.01mm/rev

0.0001inch/rev

allowed

- M29

If an S command and axis movement are specified between M29 and

G84, alarm PS0203 is issued. If M29 is specified in a tapping cycle,

alarm PS0204 is issued.

- 120 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

- Rigid tapping command M code

The M code used to specify the rigid tapping mode is set in parameter

No. 5210.

- P

Specify P in a block that performs drilling. If P is specified in a

non-drilling block, it is not stored as modal data.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G84 in a

single block. Otherwise, G84 will be canceled.

- Tool offset

In the canned cycle mode, tool offsets are ignored.

- Program restart

A program cannot be restarted during rigid tapping.

- R

The value of R must be specified in a block which performs drilling. If

the value is specified in a block which does not perform drilling, it is

not stored as modal data.

- Subprogram call

In the canned cycle mode, specify the subprogram call command

M98P_ in an independent block.

Example

Tapping axis feedrate: 1000 mm/min

Spindle speed: 1000 min^-1

Screw lead: 1.0 mm

G98 ;

Command for feed per minute

G00 X100.0 ;

Positioning

M29 S1000;

Command for specifying rigid mode

G84 Z-100.0 R-20.0 F1000 ;

Rigid tapping

G99 ;

Command for feed per rotation

G00 X100.0 ;

Positioning

M29 S1000 ;

Command for specifying rigid mode

G84 Z-100.0 R-20.0 F1.0 ;

Rigid tapping

- 121 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

4.4.2

Peck Rigid Tapping Cycle (G84 or G88)

Tapping a deep hole in rigid tapping mode may be difficult due to

chips sticking to the tool or increased cutting resistance. In such cases,

the peck rigid tapping cycle is useful.

In this cycle, cutting is performed several times until the bottom of the

hole is reached. Two peck tapping cycles are available: High-speed

peck tapping cycle and standard peck tapping cycle. These cycles are

selected using the bit 5 (PCP) of parameter No. 5200.

Format

When rigid tapping is specified with G84 (G88) if bit 5 (PCP) of

parameter No. 5200 = 0, high-speed peck rigid tapping is assumed.

G84 X(U)_ C(H)_Z(W)_ R_ P_ Q_ F_ K_ M_ ;

G88 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 the hole

: Depth of cut for each cutting feed

: The 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)

- High-speed peck rigid tapping cycle

Spindle stop

d = Amount of

Spindle stop

In the first cutting from point R, perform

return

cutting by depth "q" specified by address Q

while rotating the spindle in the forward

Mα

direction (operation <1>).

Initial level

Spindle stop

Then, perform returning by the amount

Spindle CW

Spindle stop

specified by parameter No. 5213 while

Spindle CW

Point R

Spindle CW

Point R

Spindle stop

Spindle CW

M(α+1)

Point R

level

Point R

level

M(α+1)

rotating the spindle in the reverse direction

(operation <2>).

Then, perform tapping by (d+q) while

(1)

rotating the spindle in the forward direction

(2)

(operation <3>).

(3)

Repeat operations <2> and <3> until the

bottom of the hole is reached.

Spindle stop

Spindle CCW

The cutting speed and rigid tapping time

constant are used for operations <1> and

<3>.

For operation <2> and travel from the

bottom of the hole (point Z) to point R, rigid

tapping extract override is enabled and the

Point Z

rigid tapping extract time constant is used.

Spindle stop P1

Spindle CCW

Spindle stop

Spindle CCW

- 122 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

When rigid tapping is specified with G84 (G88) if bit 5 (PCP) of

parameter No. 5200 = 1, peck rigid tapping is assumed.

G84 X(U)_ C(H)_Z(W)_ R_ P_ Q_ F_ K_ M_ ;

G88 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 the hole

: Depth of cut for each cutting feed

: The 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)

- Peck rigid tapping cycle

d = Cutting start distance

In the first cutting from point R, perform

Spindle stop

cutting by depth "q" specified by address Q

Spindle CW

while rotating the spindle in the forward

Mα

Initial level

direction (operation <1>).

Then, return to point R by rotating the

Spindle CW

Spindle stop

spindle in the reverse direction (operation

Point R

M(α+1)

Point R

M(α+1)

Point R

<2>).

level

(3)

level

(3)

Then, rotate the spindle in the forward

(1)

direction and perform cutting to the position

(2)

indicated by [(Position to which cutting was

performed previously) - (Cutting start

(4)

distance set in parameter No. 5213)] as

movement to the cutting start point

(operation <3>).

Spindle stop

Continue cutting by (d+q) (operation <4>).

Spindle CCW

Repeat operations <2> to <4> until the

bottom of the hole is reached.

The cutting speed and rigid tapping time

constant are used for operations <1> and

Point Z

<4>.

For operations <2>, <3>, and travel from

Spindle stop

Spindle CCW

Spindle stop

P1 Spindle CCW

the bottom of the hole (point Z) to point R,

rigid tapping extract override is enabled

and the rigid tapping extract time constant

The symbols in the figure above indicate the following operations.

is used.

: Positioning (Rapid traverse G00)

: Cutting feed (Linear interpolation G01)

: Dwell programmed by the address P command

Mα

: Output of the M code for C-axis clamp (The α value is set in parameter No. 5110.)

M(α+1)

: Output of the M code for C-axis unclamp

: Dwell set by parameter No.5111

Note P1, Mα, M(α+1), and P2 are not executed or output without being specified or set.

- 123 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

Explanation

- Cutting start distance

Cutting start distance d is set by parameter No. 5213.

- Amount of return

Amount of return for each time d is set by parameter No. 5213.

- Return speed

For the speed of return operation, a maximum of 2000% of override

can be enabled by setting DOV (bit 4 of parameter No. 5200), OVU

(bit 3 of parameter No. 5201), and parameter No. 5211 as with travel

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

- Speed during cutting into the cutting start point

For the speed during cutting into the cutting start point, a maximum of

2000% of override can be enabled by setting DOV (bit 4 of parameter

No. 5200), OVU (bit 3 of parameter No. 5201), and parameter No.

5211 as with travel from the bottom of the hole (point Z) to point R.

- Acceleration/deceleration after interpolation

Linear or bell-shaped acceleration/deceleration can be applied.

- Look-ahead acceleration/deceleration before interpolation

Look-ahead acceleration/deceleration before interpolation is invalid.

- Override

Various types of override functions are invalid. The following

override functions can be enabled by setting corresponding

parameters:

• Extraction override

• Override signal

Details are given later.

- Dry run

Dry run can be executed also in G84 (G88). When dry run is executed

at the feedrate for the drilling axis in G84 (G88), tapping is performed

according to the feedrate. Note that the spindle speed becomes faster

at a higher dry run feedrate.

- Machine lock

Machine lock can be executed also in G84 (G88).

When G84 (G88) is executed in the machine lock state, the tool does

not move along the drilling axis. Therefore, the spindle does not also

rotate.

- Reset

When a reset is performed during rigid tapping, the rigid tapping

mode is canceled and the spindle motor enters the normal mode. Note

that the G84 (G88) mode is not canceled in this case when bit 6 (CLR)

of parameter No. 3402 is set.

- 124 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

- Interlock

Interlock can also be applied in G84 (G88).

- Feed hold and single block

When parameter FHD (No. 5200#6) is set to 0, feed hold and single

block are invalid in the G84 (G88) mode. When this bit is set to 1,

they are valid.

- Manual feed

For rigid tapping by manual handle feed, see the section "Rigid

Tapping by Manual Handle."

With other manual operations, rigid tapping cannot be performed.

- Backlash compensation

In the rigid tapping mode, backlash compensation is applied to

compensate the lost motion when the spindle rotates clockwise or

counterclockwise. Set the amount of backlash in parameters Nos. 5321

to 5324.

Along the drilling axis, backlash compensation has been applied.

- Series 10/11 format

When bit 1 (FCV) of parameter No. 0001 is set to 1, execution is

enabled with G84.2. The same operation as with G84 is performed.

However, the command format for the repetitive count is L.

Limitation

- Axis switching

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

canceled. If the drilling axis is changed in rigid mode, alarm PS0206

is issued.

- S commands

If a speed higher than the maximum speed for the gear being used is

specified, alarm PS0200 is issued.

When the rigid tapping canned cycle is cancelled, the S command

used for rigid tapping is cleared to S0.

- Distribution amount for the spindle

The maximum distribution amount is 32,767 pulses per 8 msec for a

serial spindle. (displayed on diagnostic display No. 451)

This amount is changed according to the gear ratio setting for the

position coder or rigid tapping command. If a setting is made to

exceed the upper limit, alarm PS0202 is issued.

- 125 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

- F command

Specifying a value larger than the upper limit for cutting feed will

cause alarm PS0011 to be issued.

- Unit of F command

Metric input

Inch input

Remarks

Decimal point programming

G98

1mm/min

0.01inch/min

allowed

Decimal point programming

G99

0.01mm/rev

0.0001inch/rev

allowed

- M29

If an S command and axis movement are specified between M29 and

G84, alarm PS0203 is issued. If M29 is specified in a tapping cycle,

alarm PS0204 is issued.

- Rigid tapping command M code

The M code used to specify the rigid tapping mode is set in parameter

No. 5210.

- P/Q

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.

When Q0 is specified, the peck rigid tapping cycle is not performed.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G84 in a

single block. Otherwise, G84 will be canceled.

- Tool offset

In the canned cycle mode, tool offsets are ignored.

- Subprogram call

In the canned cycle mode, specify the subprogram call command

M98P_ in an independent block.

- d (parameter No.5213)

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).

- 126 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

4.4.3

Canned Cycle Cancel (G80)

The rigid tapping canned cycle is canceled. For how to cancel this

cycle, see II-4.3.4.

NOTE

When the rigid tapping canned cycle is cancelled,

the S value used for rigid tapping is also cleared

(as if S0 is specified).

Accordingly, the S command specified for rigid

tapping cannot be used in a subsequent part of the

program after the cancellation of the rigid tapping

canned cycle.

After canceling the rigid tapping canned cycle,

specify a new S command as required.

- 127 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

4.4.4

Override during Rigid Tapping

Various types of override functions are invalid. The following

override functions can be enabled by setting corresponding

parameters:

• Extraction override

• Override signal

4.4.4.1 Extraction override

For extraction override, the fixed override set in the parameter or

override specified in a program can be enabled at extraction (including

retraction during peck drilling/high-speed peck drilling).

Explanation

- Specifying the override in the parameter

Set bit 4 (DOV) of parameter No. 5200 to 1 and set the override in

parameter No. 5211.

An override from 0% to 200% in 1% steps can be set. Bit 3 (OVU) of

parameter No. 5201 can be set to 1 to set an override from 0% to

2000% in 10% steps.

- Specifying the override in a program

Set bit 4 (DOV) of parameter No. 5200 and bit 4 (OV3) of parameter

No. 5201 to 1. The spindle speed at extraction can be specified in the

program.

Specify the spindle speed at extraction using address "J" in the block

in which rigid tapping is specified.

Example)

To specify 1000 min^-1 for S at cutting and 2000 min^-1 for S at

extraction

M29 S1000 ;

G84 Z-100. F1000. J2000 ;

The difference in the spindle speed is converted to the actual override

by the following calculation.

Therefore, the spindle speed at extraction may not be the same as that

specified at address "J". If the override does not fall in the range

between 100% and 200%, it is assumed to be 100%.

Spindle speed at extraction (specified at

Override (% )

100

Spindle speed (specified at

)

Bit 6 (OVE) of parameter No. 5202 can be set to 1 to extend the

override value to 100% to 2000%. If the specified override value is

outside the range between 100% and 2000%, it is assumed to be

100%.

- 128 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

The override to be applied is determined according to the setting of

parameters and that in the command as shown in the table below.

When bit 6 (OVE) of parameter No. 5202 is set to 0

Parameter setting

DOV=1

DOV=0

Command

OV3=1

OV3=0

Spindle speed at extraction

Within the range between 100 to 200%

Command in

specified at address J

the program

Parameter

Within the range between 100 to 200%

100%

No. 5211

No spindle speed at extraction specified at address J

Parameter No.

5211

When bit 6 (OVE) of parameter No. 5202 is set to 1

Parameter setting

DOV=1

DOV=0

Command

OV3=1

OV3=0

Spindle speed at extraction

Within the range between 100 to 2000%

Command in

specified at address J

the program

Parameter

Within the range between 100 to 2000%

100%

No. 5211

No spindle speed at extraction specified at address J

Parameter No.

5211

NOTE

Do not use a decimal point in the value specified at address "J".

If a decimal point is used, the value is assumed as follows:

Example) When the increment system for the reference axis is IS-B

• When pocket calculator type decimal point programming is not used

The specified value is converted to the value for which the least input

increment is considered.

"J200." is assumed to be 200000 min^-1.

• When pocket calculator type decimal point programming is used

The specified value is converted to the value obtained by rounding down to an

integer.

"J200." is assumed to be 200 min^-1.

Do not use a minus sign in the value specified at address "J".

If a minus sign is used, a value outside the range is assumed to be specified.

The maximum override is obtained using the following equation so that the spindle

speed to which override at extraction is applied do not exceed the maximum used

gear speed (specified in parameters Nos. 5241 to 5244). For this reason, the

obtained value is not the same as the maximum spindle speed depending on the

override.

Maximum spindle speed (specified in

parameters

)

Maximum override (%)

100

Spindle speed (specified at

)

When a value is specified at address "J" for specifying the spindle speed at

extraction in the rigid tapping mode, it is valid until the canned cycle is canceled.

- 129 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

4.4.4.2

Override signal

By setting bit 4 (OVS) of parameter No. 5203 to 1, override can be

applied to cutting/extraction operation during rigid tapping as follows:

•

Applying override using the feedrate override signal

•

Canceling override using the override cancel signal

There are the following relationships between this function and

override to each operation:

•

At cutting

When the override cancel signal is set to 0

Value specified by the override signal

When the override cancel signal is set to 1

100%

•

At extraction

When the override cancel signal is set to 0

Value specified by the override signal

When the override cancel signal is set to 1 and extraction

override is disabled

100%

When the override cancel signal is set to 1 and extraction

override is enabled

Value specified for extraction override

NOTE

1 The maximum override is obtained using the following

equation so that the spindle speed to which override

is applied do not exceed the maximum used gear

speed (specified in parameters Nos. 5241 to 5244).

For this reason, the obtained value is not the same as

the maximum spindle speed depending on the

override.

Maximumspindle speed (specified in

parameters)

Maximum override (%)

100

Spindle speed (specified at

)

2 Since override operation differs depending on the

machine in use, refer to the manual provided by the

machine tool builder.

- 130 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

4.5

CANNED GRINDING CYCLE (FOR GRINDING MACHINE)

With the canned grinding cycle, repetitive machining operations that

are specific to grinding and are usually specified using several blocks

can be specified using one block including a G function. So, a

program can be created simply. At the same time, the size of a

program can be reduced, and the memory can be used more efficiently.

Four types of canned grinding cycles are available:

•

Traverse grinding cycle (G71)

(G72 when G code system C is used)

•

Traverse direct constant-size grinding cycle (G72)

(G73 when G code system C is used)

•

Oscillation grinding cycle (G73)

(G74 when G code system C is used)

•

Oscillation direct constant-size grinding cycle (G74)

(G75 when G code system C is used)

In the descriptions below, an axis used for cutting with a grinding

wheel and an axis used for grinding with a grinding wheel are referred

to as follows:

Axis used for cutting with a grinding wheel: Cutting axis

Axis used for grinding with a grinding wheel: Grinding axis

For a depth of cut on a cutting axis and a distance of grinding on a

grinding axis, the incremental system (parameter No. 1013) for the

reference axis (parameter No. 1031) is used. If 0 is set in parameter

No. 1031 (reference axis), the incremental system for the first axis is

used.

NOTE

The canned grinding cycle is an optional function.

The canned grinding cycle and multiple repetitive

cycle cannot be used simultaneously for the same

path.

To use the canned grinding cycle, set bit 0 (GFX)

of parameter No. 5106 to 1.

- 131 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

WARNING

The G codes for canned grinding cycles G71,

G72, G73, and G74 (G72, G73, G74, and G75

when G code system C is used) are G codes of

group 01. A G code for cancellation such as G80

used for a canned cycle for drilling is unavailable.

By specifying a G code of group 00 other than

G04, modal information such as a depth of cut is

cleared but no canned grinding cycle can be

canceled. To cancel a canned grinding cycle, a G

code of group 01 other than G71, G72, G73, and

G74 needs to be specified. So, when switching to

another axis move command from G71, G72, G73

or G74, for example, be sure to specify a G code

of group 01 such as G00 or G01 to cancel the

canned grinding cycle. If another axis move

command is specified without canceling the

canned grinding cycle, an unpredictable operation

can result because of continued cycle operation.

NOTE

If the G code for a canned grinding cycle (G71,

G72, G73, or G74) is specified, the canned

grinding cycle is executed according to the values

of A, B, W, U, I, and K preserved as modal data

while the cycle is valid, even if a block specified

later specifies none of G71, G72, G73, and G74.

Example:

G71 A_ B_ W_ U_ I_ K_ H_ ;

;

← The canned grinding cycle is executed

even if an empty block is specified.

When switching from a canned cycle for drilling to

a canned grinding cycle, specify G80 to cancel

the canned cycle for drilling.

When switching from a canned grinding cycle to

another axis move command, cancel the canned

cycle according to the warning above.

A canned grinding cycle and multiple repetitive

canned cycle cannot be used simultaneously on

the same path.

When the canned grinding cycle option is enabled,

which function is to be used can be selected using

bit 0 (GFX) of parameter No. 5106.

- 132 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

4.5.1

Traverse Grinding Cycle (G71)

A traverse grinding cycle can be executed.

Format

G71 A_ B_ W_ U_ I_ K_ H_ ;

A_ : First depth of cut (The cutting direction depends on the sign.)

B_ : Second depth of cut (The cutting direction depends on the sign.)

W_ : Grinding range (The grinding direction depends on the sign.)

U_ : Dwell time

: Feedrate for A and B

K_ : Feedrate for W

H_ : Repetitive count (from 1 to 9999)

G71

<1>(I)

<3>(K)

<2>U

<4>(I)

<6>(K)

<5>U

- 133 -

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Lathe System USER’S MANUAL - page 5