14. FUNCTIONS TO SIMPLIFY
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
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 K 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.
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
In a block that does not contain X, Y, Z, R, or any other axes, drilling is
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 G99 G73 X300. Y–250. Z–150. R–100. Q15. 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
G80 G28 G91 X0 Y0 Z0 ; Return to the reference position return
M5 ; Cause the spindle to stop rotating.
D Axis switching
D Tool offset