What model Fanuc is this for?
According to the Fanuc Mill operator's manual (0i-B/C) macros called by G-codes are simple only (G65), not modal (G66). I assume this holds true throughout other models.
Hi
So i have created my own drilling cycle and instead of using G66 Pxxxx i want to use G810.
My issue is that it wont excecute the cycle on the next hole.
Example
G810 x10y0 <-- this one works
x20y0 <- no cycle here
G80 <-- also not sure if G80 would work?
What do i need to put in the sub program? And is this even possible?
Similar Threads:
What model Fanuc is this for?
According to the Fanuc Mill operator's manual (0i-B/C) macros called by G-codes are simple only (G65), not modal (G66). I assume this holds true throughout other models.
It appears that Fanuc has included the ability to call modal macros from G-codes on the 31i (see attached)
Thank you that worked
However it gave me another issue, when going to the next coordinate it doesn't remember the values, so i put them all in other variables and i will skip adding them again when moving to the next coordinate, but i if i wanna change depth of the next hole this doesn't really work. Any suggestions?
In time i will add some pecking options to it
O9810(LONGDRILL-CYCLE)
(G810 R5 Z-150. E50 F230 S800)
(R=SAFETY PLANE)
(Z=DEPTH)
(E=PREDRILL POINT)
IF[#7 EQ 80]GOTO9999
IF[#120 EQ 1]GOTO10
#120=1(FIRST TIME CALL)
#111=#5003(CURRENT Z)
#110=#4119(CURRENT S)
#100=#18(R)
#101=#19(S)
#102=#9(F)
#103=#8(E)
#104=#26(Z)
IF[#8LT20]THEN#3000=1(-E-MUST-BE-BIGGER-THAN 20)
IF[#110LT1]THEN#3000=1(NEED SOME SPEED WHILE ENGAGING)
N10
S#110M3
G0Z#100
G1Z[#100-#103+5]F500
M88(COOLANT ON)
G04X0.2
S[#101/2]
G1Z[#100-#103-10]F[#102/2]
G1Z[#5003+0.2]
S#101
G4X0.5
G1Z#104F#102
G1Z[#5003+0.2]
G4X0.5
S#110M3
M89(COOLANT OFF)
Z#100F1000
G0Z#111
M99
N9999
#199=0
G67
%