CNC program example for cnc vertical machining centers illustrates the use of G81 drilling cycle.
CNC milling machine controls like Fanuc, Haas etc, has many standard canned cycles built-in the cnc control, these canned cycles make the cnc programmer/ setter/ operator’s life easier as canned cycles are easy to program and debug.
O10075 N1 T16 M06 N2 G90 G54 G00 X0.5 Y-0.5 N3 S1450 M03 N4 G43 H16 Z1. M08 N5 G81 G99 Z-0.375 R0.1 F9. N6 X1.5 N7 Y-1.5 N8 X0.5 N9 G80 G00 Z1. M09 N10 G53 G49 Z0. M05 N11 M30
O10075 Program number (there are many programs in cnc memory so they are distinguished by their number).
N1- Tool change (M06) to tool no.16
N2- Tool rapidly moves (G00) to first drilling position X0.5 Y-0.5 while taking into account Zero-offset-no. 1 (G54)
N3- Drill starts rotating clockwise (M03) with 1450 rpm (S1450).
N4- Drill takes depth Z1. taking into account tool length compensation (G43 H16), coolant is turned on (M08).
N5- Drilling cycle (G81) parameters, drill depth (Z) and cutting feed (F) are given, with this command first drill is made at current position (X0.5 Y-0.5).
N6- As drilling cycle continues it’s work with every axis movement so next drill is done at X1.5
N7- Third drilling hole at Y-1.5
N8- Fourth drill at X0.5
N9- Drilling cycle is canceled (G80), Coolant is turned off (M09).
N10- Taking Machine-coordinate-system (G53) into account the drill is taken to Z0 position. Tool length compensation is canceled (G49), cutter rotation is stopped (M05).
N11- CNC part-program is ended.
G & M Codes
|T||Tool no. used.|
|M06||Tool change command.|
|G54||Zero offset no.1|
|M03||Cutter rotation Clockwise|
|G43||Tool length compensation.|
|G81||Fanuc drilling cycle.|
|G80||Canned cycle cancel.|
|G53||Machine coordinate system selection.|
|G49||Tool length compensation cancel.|
|M05||Cutter rotation stop.|
|M30||CNC part-program end.|