FANUC Series 16/18/160/180-Model C Machining Center Operators Manual

PROGRAMMING
B–62764EN/01
14. FUNCTIONS TO SIMPLIFY
PROGRAMMING
201
After positioning along the X– and Y–axes, the spindle is stopped at the
fixed rotation position. The tool is moved in the direction opposite to the
tool tip, positioning (rapid traverse) is performed to the bottom of the hole
(point R).
The tool is then shifted in the direction of the tool tip and the spindle is
rotated clockwise. Boring is performed in the positive direction along the
Z–axis until point Z is reached.
At point Z, the spindle is stopped at the fixed rotation position again, the
tool is shifted in the direction opposite to the tool tip, then the tool is
returned to the initial level. The tool is then shifted in the direction of the
tool tip and the spindle is rotated clockwise to proceed to the next block
operation.
Before specifying G87, use a miscellaneous function (M code) to rotate
the spindle.
When the G87 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 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
canceled.
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 No.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 G87 X300. Y–250. Position, bore hole 1.
Z–150. R–120. Q5. Orient at the initial level, then shift by 5 mm.
P1000 F120. ; Stop at point Z for 1 s.
Y–550. ; Position, drill hole 2.
Y–750. ; Position, drill hole 3.
X1000. ; Position, drill hole 4.
Y–550. ; Position, drill hole 5.
Y–750. ; Position, drill hole 6
G80 G28 G91 X0 Y0 Z0 ; Return to the reference position return
M5 ; Cause the spindle to stop rotating.
Explanations
Restrictions
D Axis switching
D Boring
D Q/R
D Cancel
D Tool offset
Examples

Leave a Reply

Your email address will not be published.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