Fanuc Power Mate i-D/H Operator Manual

2. FUNCTION TO SIMPLIFY
PROGRAMMING
PROGRAMMING
(For the Power Mate i–D/D2)
B–63174EN/03
183
The high–speed peck drilling cycle performs intermittent feeding along
the Z–axis. When this cycle is used, chips can be removed from the hole
easily, and a smaller value can be set for retraction. This allows, drilling
to be performed efficiently. Set the clearance, d, in parameter 5114.
The tool is retracted in rapid traverse.
Before specifying G73, rotate the spindle using a miscellaneous function
(M code).
When the G73 code and an M code are specified in the same block, the
M code is executed at the time of the first positioning operation. The
system then proceeds to the next drilling operation.
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.
Before the drilling axis can be changed, the canned cycle must be
canceled.
In a block that does not contain X, Z, R, or any other axes, drilling is not
performed.
Specify Q and R in blocks that perform drilling. If they are specified in
a block that does not perform drilling, they cannot be stored as modal data.
Do not specify a group 01 G code (G00 to G03) and G73 in the same block.
If they are specified together, G73 is canceled.
In the canned cycle mode, tool offsets are ignored.
M3 S2000 ; Cause the spindle to start rotating.
G90 G73 X300. Z–150. R–100. Q15. F120. ;
Position, drill hole 1, then return to initial level.
X1000. ; Position, drill hole 2, then return to initial level.
G80 G28 G91 X0 Z0 ; Return to the reference position return
M5 ; Cause the spindle to stop rotating.
Explanations
Limitations
Axis switching
Drilling
Q/R
Cancel
Tool offset
Examples

Leave a Reply

Your email address will not be published.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