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

PROGRAMMING
16. CUSTOM MACRO
B–62764EN/01
396
G65 P9100 X x Y y Z z R r F f I i A a B b H h ;
X: X coordinate of the center of the circle
(absolute or incremental specification)(#24)
Y: Y coordinate of the center of the circle
(absolute or incremental specification)(#25)
Z: Hole depth (#26)
R: Coordinates of an approach point (#18)
F : Cutting feedrate (#9)
I : Radius of the circle (#4)
A: Drilling start angle(#1)
B: Incremental angle (clockwise when a negative value is specified)
(#2)
H: Number of holes (#11)
O0002;
G90 G92 X0 Y0 Z100.0;
G65 P9100 X100.0 Y50.0 R30.0 Z–50.0 F500 I100.0 A0 B45.0 H5;
M30;
O9100;
#3=#4003;
Stores G code of group 3.
G81 Z#26 R#18 F#9 K0; (Note) Drilling cycle..
Note: L0 can also be used.
IF[#3 EQ 90]GOTO 1; Branches to N1 in the G90 mode.
#24=#5001+#24; Calculates the X coordinate of the center.
#25=#5002+#25; Calculates the Y coordinate of the center.
N1 WHILE[#11 GT 0]DO 1;
Until the number of remaining holes reaches 0. .
#5=#24+#4*COS[#1];Calculates a drilling position on the X–axis.
#6=#25+#4*SIN[#1]; Calculates a drilling position on the Y–axis.
G90 X#5 Y#6; Performs drilling after moving to the target position.
#1=#1+#2; Updates the angle.
#11=#11–1; Decrements the number of holes.
END 1;
G#3 G80;
Returns the G code to the original state.
M99;
Meaning of variables:
#3: Stores the G code of group 3.
#5: X coordinate of the next hole to drill
#6: Y coordinate of the next hole to drill
D Calling format
D Program calling a macro
program
D Macro program
(called program)

Leave a Reply

Your email address will not be published.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