14. FUNCTIONS TO SIMPLIFY
Tapping is performed by rotating the spindle clockwise. When the bottom
of the hole has been reached, the spindle is rotated in the reverse direction
for retraction. This operation creates threads.
Feedrate overrides are ignored during tapping. A feed hold does not stop
the machine until the return operation is completed.
Before specifying G84, use a miscellaneous function (M code) to rotate
When the G84 command 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 the K is used to specify 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 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.
Do not specify a group 01 G code (G00 to G03) and G84 in the same block.
If they are specified together, G84 is canceled.
In the canned cycle mode, tool offsets are ignored.
M3 S100 ; Cause the spindle to start rotating.
G90 G99 G84 X300. Y–250. Z–150. R–120. P300 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