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

13.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63324EN/03
- 296 -
- 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.
Restriction
- Axis switching
Before the drilling axis can be changed, the canned cycle must be
canceled.
- Drilling
In a block that does not contain X, Y, Z, R, or any other axes, drilling is
not performed.
- R
Specify R in blocks that perform drilling. If it is specified in a block
that does not perform drilling, it cannot be stored as modal data.
- Cancel
Do not specify a G code of the 01 group (G00 to G03 or etc.) and G81
in a single block. Otherwise, G81 will be canceled.
- Tool offset
In the canned cycle mode, tool offsets are ignored.
Example
M3 S2000 ; Cause the spindle to start rotating.
G90 G99 G81 X300. Y-250. Z-150. R -100. F120. ;
Position, drill hole 1, then return to point R.
Y-550. ; Position, drill hole 2, then return to point R.
Y-750. ; Position, drill hole 3, then return to point R.
X1000. ; Position, drill hole 4, then return to point R.
Y-550. ; Position, drill hole 5, then return to point R.
G98 Y-750. ; Position, drill hole 6, then return to the initial level.
G80 G28 G91 X0 Y0 Z0 ; Return to the reference position return
M5 ; Cause the spindle to stop rotating.

Leave a Reply

Your email address will not be published.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