CNC G81 Drilling Cycle Program Example

Fanuc G81 drilling cycle is used for simple drilling operations, so here is a cnc program example which demonstrates how G81 drilling cycle can be used.

CNC Program

Fanuc G81 Drilling Cycle Example Program

Fanuc G81 Drilling Cycle Example Program

N1 T1 M06
N2 G90 G54 G00 X.3 Y1.2
N3 S1200 M03
N4 G43 H01 Z1. M08
N5 G81 Z-.6 R.1 F10
N6 X1.2 Y.3
N7 G80 G00 Z1. M09
N8 G28 G91 Z0. M05
N9 M30


Once G81 drilling canned cycle is defined, the canned cycle is repeated at every X-Y position in sequential blocks, G80 code is used to cancel G81 drilling cycle.

N1- Tool change to tool no.1

N2- Tool rapidly moves to first drilling position X0.3 Y1.2 while taking into account Zero-offset-no. 1

N3- Drill starts rotating clockwise with 1200 rpm.

N4- Drill takes depth Z1. taking into account tool length compensation (G43 H01), coolant is turned on.

N5- Drilling cycle parameters, drill depth and cutting feed are given, with this command first drill is made at current position (X0.3 Y1.2).

N6- As drilling cycle continues it’s work with every axis movement so next drill is done at X1.2 Y0.3

N7- Drilling cycle is canceled with G80 command, Coolant is turned off.

N8- As operation for this component is finished, so cutting tool is taken to reference position, and cutter rotation is stopped.

N9- CNC part-program is ended.

G & M Codes

TTool no. used.
M06Tool change command.
G90Absolute programming
G54Zero offset no.1
G00Rapid traverse
SCutter speed
M03Cutter rotation Clockwise
G43Tool length compensation.
M08Coolant on.
G81Fanuc drilling cycle.
FCutting feed.
G80Canned cycle cancel.
M09Coolant off.
G28Return to reference position.
G91Incremental programming.
M05Cutter rotation stop.
M30CNC part-program end with return to program-start.