Create a Custom G81 Drilling Cycle Using Fanuc Macro and G66 Modal Call

This is a complete Fanuc Macro which works same as Fanuc G81 Drilling Cycle.

Create a Custom G81 Drilling Cycle Using Fanuc Macro and G66 Modal Call Image: directindustry.com

G66 Modal Call

Once Fanuc G66 is issued to specify a modal call a macro is called after a block specifying movement along axes is executed. This continues until G67 is issued to cancel a modal call.

Macro Call Parameters

G65 P9110 X x Y y Z z R r F f L l ;

X: X coordinate of the hole (absolute only) . . . (#24)
Y: Y coordinate of the hole (absolute only) . . . (#25)
Z: Coordinates of position Z (absolute only). . . (#26)
R: Coordinates of position R (absolute only). . . (#18)
F : Cutting feedrate . . . . . . . . . . . . . . . . . . . .. . . (#9)
L: Repetition count

Program Example

O0001;
G28 G91 X0 Y0 Z0;
G92 X0 Y0 Z50.0;
G00 G90 X100.0 Y50.0;
G66 P9110 Z–20.0 R5.0 F500;
G90 X20.0 Y20.0;
X50.0;
Y50.0;
X70.0 Y80.0;
G67;
M30;

Drilling Macro

O9110;
#1=#4001; 		(Stores G00/G01)
#3=#4003; 		(Stores G90/G91)
#4=#4109; 		(Stores the cutting feedrate)
#5=#5003; 		(Stores Z coordinate at the start of drilling)
G00 G90 Z#18; 		(Positioning at position R)
G01 Z#26 F#9; 		(Cutting feed to position Z)
IF[#4010 EQ 98]GOTO 1; 	(Return to position I)
G00 Z#18; 		(Positioning at position R)
GOTO 2;
N1 G00 Z#5; 		(Positioning at position I)
N2 G#1 G#3 F#4; 	(Restores modal information)
M99;

Comprehensive Fagor 800M & 800T G‑Codes & M‑Codes Guide Complete G Codes & M Codes Guide for Fagor 101/102 CNC Systems

CNC Machine

Industrial robot

Industrial equipment