14. FUNCTIONS TO SIMPLIFY
When the bottom of the hole has been reached, the spindle is stopped at
the fixed rotation position, and the tool is moved in the direction opposite
to the tool tip and retracted. This ensures that the machined surface is not
damaged and enables precise and efficient boring to be performed.
Before specifying G76, use a miscellaneous function (M code) to rotate
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. The
system then proceeds to the next 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 additional axes, boring
is not performed.
Be sure to specify a positive value in Q. If Q is specified with a negative
value, the sign is ignored. Set the direction of shift in bits 4 (RD1) and
5 (RD2) of parameter 5101. Specify Q and R in a block that performs
boring. If they are specified in a block that does not perform boring, they
are not stored as modal data.
Do not specify a group 01 G code (G00 to G03) and G76 in the same block.
If they are specified together, G76 is canceled.
In the canned cycle mode, tool offsets are ignored.
M3 S500 ; Cause the spindle to start rotating.
G90 G99 G76 X300. Y–250.
Position, bore hole 1, then return to point R.
Z–150. R–120. Q5. Orient at the bottom of the hole, then shift
by 5 mm.
P1000 F120. ; Stop at the bottom of the hole for 1 s.
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