Fanuc controls do not have the very useful G12 and G13 circular pocketing cycle as a standard feature. Controls that do have it, for example Yasnac, have a built-in macro (cycle), ready to be used. Fanuc users can create their own custom macro (as a special G-code cycle), with the optional User Macro (Custom Macro) feature, which can be developed to offer even more flexibility than a built-in cycle.
The codes also same as for Mitsubishi CNC controller. Circular cutting starts the tool from the center of the circle, and cuts the inner circumference of the circle. The tool continues cutting while drawing a circle and returns to the center position.
The two G-codes are identical in all respects, except the cutting direction. Meaning of the two G-codes in a circular pocket cycle is:
G12 : Circular pocket cutting CW
G13 : Circular pocket cutting CCW
Either cycle is always programmed without cutter radius offset in effect - in G40 cancel mode - and has the following program format:
G12 I… D… F… ; (Conventional Milling)
G13 I… D… F… ; (Climb Milling)
I = Pocket radius
D = Cutter radius offset number
F = Cutting feedrate
Typically, either cycle is called in a program when cutting tool reaches the center and the bottom of a pocket to be machined. All cutting motions are arc motions, and there are three of them. There are no linear motions. The arbitrary start point (and end point) on the pocket diameter will usually be at 0 degree (3 o’clock) - Figure 33-16.
Circular pocket cycles G12 and G13
If G12 or G13 cycle or a similar macro is available, the following program O3306 can be written, using the same tool and climb milling mode:
O3306 (CIRCULAR POCKET - G13 EXAMPLE) N1 G20 N2 G17 G40 G80 N3 G90 G54 G00 X0 Y0 S1200 M03 N4 G43 Z0.1 H01 M08 N5 G01 Z-0.25 F8.0 N6 G13 I0.75 D1 F10.0 (CIRCULAR POCKET) N7 G28 Z-0.25 M09 N8 G91 G28 X0 Y0 M05 N9 M30
G12 I50.000 D01 F100 ; When compensation amount is +10.000mm