640m g-code

[lx545]

I have a 640m fusion control on a 655/80n mill and Im trying to run a eia subprogram in a mazatrol program. I have the program correct accept it does not recognize the dia of the tool in mazatrol its working kind of like a line center if that helps. I set the f94 and two other parameters and tryed offsetting but Im not real familiar with what to do, and help? thanks

[Mazachist]

The machine is set up to use tool data for mazatrol programs and tool offsets for g code programs. You may need a G43 Hxx and G41 or G42 Dxx in your program. Restarting your machine after changing F94 bit 7 may be necessary.

YO

[jimiscnc]

Mazak gives EIA programmers a choice for TLC and CRC - do it standard G code way (aka "fanuc way") or do it the very elegant "Mazak way", as described below.

CRC:
CRC with D offset register: F92.7 = 1 (D word uses EIA offset registers)
CRC by "mazak way" F92.7=0 (uses Mazatrol TOOL DATA and offsets path by ACT-DIA)/2 in Mazatrol Tool Data. Still need G41/42 but D word not required

TLC:
TLC with G43 and H word: F93.3=0 (H word uses EIA offset registers)
TLC by "Mazak way"" F93.3=1 (tool length "goes with the tool" in and out of the spindle and stays in the coordinate system until tool change. Tool length value is in Tool Data page)

Note: RESET will wipe out EIA type using G43, RESET DOES NOT wipe out mazatrol way!

from notes. be forewarned; I did too much acid back in my hippy days!

-jim

PS - F94.7 is the switch for using H/D or not. I prefer Mazak way greatly, so I don't use F94 much.