Fanuc Series 15i/150i-MA (Programming) Operators Manual

- 293 -
- Miscellaneous function
When the G76 command and an M code are specified in the same block,
the M code is executed at the time of the first positioning operation.
When L is used to specify the number of repeats, the M code is
executed for the first hole only; for the second and subsequent holes,
the M code is not executed.
- Tool length compensation
When a tool length offset (G43, G44, or G49) is specified in the canned
cycle, the offset is applied at the time of positioning to point R.
- Shift specification by I_J_
When bit 2 (SIJ) of parameter No. 6200 is set to 1, specify a shift with
I_J_. Specify a shift for each positioning plane as described below.
Assume the following:
Xp : X-axis or axis parallel with the X-axis
Yp : Y-axis or axis parallel with the Y-axis
Zp : Z-axis or axis parallel with the Z-axis
Then, specify a shift as follows:
G17 (XpYp plane): Use I and J for specification.
G18 (ZpXp plane): Use K and I for specification.
G19 (YpZp plane): Use J and K for specification.
For example, when the XY plane is selected, a shift is made with linear
interpolation along the X- and Y-axes by the incremental value
specified by I and J. This means that a shift is made in an arbitrary
direction on the positioning plane. The feedrate specified in F is used.
I, J, and K are modal in a canned cycle. Specify I, J, and K in a block
containing hole position data.
- Shift specification by Q_
When bit 2 (SIJ) of parameter No. 6200 is set to 0, specify a shift with
Q_. Specify a positive value for Q. If a negative value is specified, the
sign is ignored. Set the shift direction, +X, -X, +Y, or -Y, in parameter
No. 6240 beforehand.
Q (shift at the bottom of a hole) is modal information in
a canned cycle, and is also used to specify a depth of
cut with G73 and G83.
G76 can be used only when canned cycle II is set (bit 0
(FXB) of parameter No. 6201 is set to 1).

Leave a Reply

Your email address will not be published. Required fields are marked *