Is it possible to manually program diameter offset?

Is it possible to manually program diameter offset?

Answer
 
Comments 0

2 Answers

Yes, in the days before cutter compensation... everything was programmed to tool center. Painful times...

 
Comments 0

Yes, brief discription first.

In most Fanuc controls, G41 & G42 compensates the tool to the left (G41) right (G42) when programming in "1/2 Comp" lead in length must be greater than the Comp applied. A "D(number)" is needed to know where to read the offset value from. T1 = D41 and T2 = D42

If you use half comp, your toolpath is the part shape, so using a Ø.50 endmill your comp value would be .250 (radius of tool).
At "zero comp", your toolpath includes the radial offset. Comp value in turn would be Zero.

Half comp needs cutter comp. Zero comp doesn't but should anyway.
Here I have an example of a Ø.50 endmill cutting the same 1"x1" square.
First using half comp, second Zero comp, third zero comp with cutter comp added (what your requesting).

(HALF COMP)

G0X0.Y7.
G0G90G54X-.5Y1.B0.
G43H1Z4.
Z.1
G1Z0.F10.
G41D41Y.5 <-- G41 TURNS ON COMP D41=VALUE TO OFFSET .250
X.5
Y-.5
X-.5
Y.5
G40X-1. <-- G40 TURNS OFF COMP
G0Z4.

(ZERO COMP)
(NO CUTTERCOMP)

G0X0.Y7.
G0G90G54X-.75Y1.25B0.
G43H1Z4.
Z.1
G1Z0.F10.
Y.75
X.75
Y-.75
X-.75
Y.75
X-1.25
G0Z4.

(ZERO COMP)
(WITH CUTTERCOMP)

G0X0.Y7.
G0G90G54X-.75Y1.25B0.
G43H1Z4.
Z.1
G1Z0.F10.
G41D41Y.75 <-- G41 TURNS ON COMP D41=VALUE TO OFFSET 0
X.75
Y-.75
X-.75
Y.75
G40X-1.25 <-- G40 TURNS OFF COMP
G0Z4.

 
Comments 0