FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 22

4.INTERPOLATION FUNCTIONS

PROGRAMMING

B-63944EN/03

- 132 -

Limitation
- Manual operation

The hypothetical axis can be used only in automatic operation. In
manual operation, it is not used, and movement takes place.

- Move command

Specify hypothetical axis interpolation only in the incremental mode.

- Coordinate rotation

Hypothetical axis interpolation does not support coordinate rotation.

Example
- Sine interpolation

20.0

10.0

N001 G07 X0 ;
N002 G91 G17 G03 X-20.0 Y0.0 I-10.0 Z20.0 F100 ;
N003 G01 X10.0 ;
N004 G07 X1 ;
From the N002 to N003 blocks, the X-axis is set to a hypothetical axis.
The N002 block specifies helical cutting in which the Z-axis is the
linear axis. Since no movement takes place along the X axis,
movement along the Y-axis is performed while performing sine
interpolation along the Z-axis.
In the N003 block, there is no movement along the X-axis, and so the
machine dwells until interpolation terminates.

- Changing the feedrate to form a sine curve

(Sample program)
G07Z0 ;

The Z-axis is set to a hypothetical axis.

G02X0Z0I10.0F4. ; The feedrate on the X-axis changes sinusoidally.
G07Z1 ;

The use of the Z-axis as a hypothetical axis is

canceled.

4.0

B-63944EN/03

PROGRAMMING

4.INTERPOLATION FUNCTIONS

- 133 -

4.16

VARIABLE LEAD THREADING (G34)

Specifying an increment or a decrement value for a lead per screw
revolution enables variable lead threading to be performed.

Fig. 4.16 (a) Variable lead screw

Format

G34

_ F_ K_ Q_ ;

_ : End point

F_  : Lead in longitudinal axis direction at the start point
K_  : Increment and decrement of lead per spindle revolution
Q_  : Shift amount of starting angle of thread cutting

Explanation

Address other than K are the same as in straight/taper thread cutting
with G32.
The K value depends on the increment system of the reference axis, as
indicated in Table 4.16 (a).
If the specified K value exceeds the range indicated in Table 4.16 (a),
if the maximum lead is exceeded after a change due to the K value, or
if the lead value is negative, an alarm PS0313 will be issued.

Table 4.16 (a) Range of valid K values

Increment system

of reference axis

Metric input (mm/rev)

Inch input (inch/rev)

IS-A

0.001 to

500.000

0.00001 to

50.00000

IS-B

0.0001 to

500.0000

0.000001 to

50.000000

IS-C

0.00001 to

50.00000

0.0000001 to

5.0000000

IS-D

0.000001 to

5.000000

0.00000001 to

0.50000000

IS-E

0.0000001 to

0.5000000

0.000000001 to

0.050000000

CAUTION

The "thread cutting cycle retract" is not effective for
G34.

Example

Lead at the start point: 8.0 mm
Lead increment: 0.3 mm/rev

G34 Z-72.0 F8.0 K0.3 ;

4.INTERPOLATION FUNCTIONS

PROGRAMMING

B-63944EN/03

- 134 -

4.17

CIRCULAR THREADING (G35, G36)

Using the G35 and G36 commands, a circular thread, having the
specified lead in the direction of the major axis, can be machined.

L: Lead

Fig. 4.17 (a) Circular threading

Format

A sample format for the G18 plane (Z-X plane) is indicated below.
When using the format for the G17 plane (X-Y plane), change the
addresses Z, X, K, and I to X, Y, I, and J respectively. When using the
format for the G19 plane (Y-Z plane), change the addresses Z, X, K,
and I to Y, Z, J, and K respectively.

G35 I_

G36

X_ Z_

F_ Q_ ;

G35  : Clockwise circular threading command
G36  : Counterclockwise circular threading command

X, Z  : Specify the arc end point (in the same way as for

G02, G03).

I, K : Specify the arc center relative to the start point, using

relative coordinates (in the same way as for G02,
G03).

: Specify the arc radius.

: Specify the lead in the direction of the major axis.

: Specify the shift of the threading start angle

(0° to 360°, with least input increment of 0.001)

(The value can be programmed with a decimal point.)

B-63944EN/03

PROGRAMMING

4.INTERPOLATION FUNCTIONS

- 135 -

G35 I_

G36

X(U)_ Z(W)_

F_ Q_ ;

G35 : Clockwise circular threading command
G36 : Counterclockwise circular threading command

X(U), Z(W) : Specify the arc end point (in the same way as

for G02, G03).

I, K : Specify the arc center relative to the start point, using

relative coordinates (in the same way as for G02,
G03).

: Specify the arc radius.

: Specify the lead in the direction of the major axis.

: Specify the shift of the threading start angle

(0° to 360°, with least input increment of 0.001)

(The value cannot be programmed with a decimal

point.)

End point (Z, X)

Arc center

Start point

Explanation
- Specifying the arc radius

If R is specified with I and K, only R is effective.

- Shift angle

If an angle greater than 360

is programmed, it is set to 360

- Specifying shift angle Q

To specify the shift angle Q, set bit 0 (GQS) of parameter No. 3451 to
1.

4.INTERPOLATION FUNCTIONS

PROGRAMMING

B-63944EN/03

- 136 -

- Automatic tool compensation

The G36 command is used to specify the following two functions:
Automatic tool compensation X and counterclockwise circular
threading. The function for which G36 is to be used depends on bit 3
(G36) of parameter No. 3405.

•

When parameter G36 is set to 0, the G36 command is used for
automatic tool compensation X.

•

When parameter G36 is set to 1, the G36 command is used for
counterclockwise circular threading.

G37.1 can be used to specify automatic tool compensation X and
G37.2 can be used to specify automatic tool compensation Z.
(Specification

method)

G37.1 X_

G37.2 Z_

•

G code when parameter G36 (bit 3 of No. 3405) is set to 1

G code

G code group

Function

G35

Clockwise circular threading

G36

Counterclockwise circular threading

G37

Automatic tool compensation Z

G37.1

Automatic tool compensation X

G37.2

Automatic tool compensation Z

B-63944EN/03

PROGRAMMING

4.INTERPOLATION FUNCTIONS

- 137 -

Limitation
- Range of specifiable arc

An arc must be specified such that it falls within a range in which the
major axis of the arc is always the Z-axis or always the X-axis, as
shown in Fig. 4.17 (b), and (c). If the arc includes a point at which
the major axis changes from the X-axis to Z-axis, or vice versa, as
shown in Fig. 4.17 (d), an alarm PS5058 is issued.

Start point

End point

Fig. 4.17 (b) Range in which the Z-axis is the major axis

Start point

End point

Fig. 4.17 (c) Range in which the X-axis is the major axis

Start point

End point

The major axis changes at this point.

Fig. 4.17 (d) Example of arc specification which causes an alarm

4.INTERPOLATION FUNCTIONS

PROGRAMMING

B-63944EN/03

- 138 -

- End point not on an arc

If the end point is not on an arc, a movement on an axis is made to a
position of which coordinate matches the corresponding coordinate of
the end point. Then, a movement is made on another axis to reach the
end point.

Start point

Center

End point

Center

End point

Start point

Fig. 4.17 (e) Movement when the end point is not on an arc

B-63944EN/03

PROGRAMMING

4.INTERPOLATION FUNCTIONS

- 139 -

4.18

SKIP FUNCTION (G31)

Linear interpolation can be commanded by specifying axial move
following the G31 command, like G01. If an external skip signal is
input during the execution of this command, execution of the
command is interrupted and the next block is executed.
The skip function is used when the end of machining is not
programmed but specified with a signal from the machine, for
example, in grinding. It is used also for measuring the dimensions of a
workpiece.

Format

G31

;

G31 : One-shot G code (If is effective only in the block in

which it is specified)

Explanation

The coordinate values when the skip signal is turned on can be used in
a custom macro because they are stored in the custom macro system
variable #100151 to #100182, as follows. For systems with up to 20
axes, FS16-compatible system variables (#5061 to #5080) may also be
used.

#100151 (#5061) : First axis coordinate value

#100151 (#5062) : Second axis coordinate value

#100170 (#5080) : 20th axis coordinate value

#100171

: 21st axis coordinate value

#100172

: 22nd axis coordinate value

#100182

: 32nd axis coordinate value

CAUTION

Disable feedrate override, dry run, and automatic
acceleration/deceleration (however, these become
available by setting bit 7 (SKF) of parameter
No.6200 to 1.) when the feedrate per minute is
specified, allowing for an error in the position of the
tool when a skip signal is input. These functions are
enabled when the feedrate per rotation is specified.

NOTE

If G31 command is issued while tool radius/tool
nose radius compensation is applied, an alarm
PS0035 is displayed. Cancel the tool radius
compensation with the G40 command before the
G31 command is specified.

Content .. 20 21 22 23 ..