[WonderY]

Hello, we just got an old takisawa lathe machine with live tooling. it uses Fanuc 21-T control. i can't seem to find the proper way to program the live tooling. I'm trying to mill a 0.75" square using a 0.50" dia end mill. could someone please give me an example to the actual program to do this? or how to do it? i would really appreciate the help.

thank you

[yoshi900]

i have a takisawa with live tooling also. This is something my camworks post puts out, with a little bit of hand edit on the starting rapid position.

T0101 M76
G0 G98 G20 G40
G28 C0
G97 S3000 M3
X1. Z1.
G112
G1 X-.5 C1.125 F40.
M8
Z.1
Z-.1 F10.
X-.5 C.875 F18.
G3 X0 C.625 R.25
G1 X1.25
C-.625
X-1.25
C.625
X0
G3 X.5 C.875 R.25
G1 C1.125
Z.1 F40.
G113
G0 Z1.
M9
G28 U0 W0 C0 M5
M01

G112 is "polar coordinate milling". once in G112, you don't have to figure out the complicated spindle C angle relative to X in order to make the shape. G112 makes it work like X,Y on a vertical mill (except X is express in diameter, and Y is replaced with "C")
do not use G0 when inside G112, it will alarm. Feedrate is limited to like 45 ipm. the closer x gets to 0, the faster the chuck has to spin to keep up with a constant feedrate. so you will see it spin like hell, and there is a limit and it will alarm if too fast. never have the toolpath cross the x0y0 point, chuck will have to spin at infinite rate and it will alarm for sure.

G113 gets you out of this mode and you can rapid again.

post more questions if needed.

[zavateandu]

?

[WonderY]

thank you yoshi, i will give it a try