[Lizz]

hi all,
I am currently working with the OKUMA LB3000 2 spindles live tools and I'm lost on how to make the "D" compensation on this machine, since this is not a mill, I know its something related to the "R" radius of tool.
The piece I am working on its cylindrical and have 10 irregular windows on the circumference. I made the programs with CAMWORKS, everything was ok the machining is good, except for the part that I DON KNOW HOW TO MAKE THE COMPENSATIONS and I obviously need to be able to do them because the finish tools don't always have the same diameters and because of the wear off. PLEASE HELP ME

the program works using the C-Z axis movement only, like this:
O2(SUB FOR FINISH)
G01 X2.460 F8.0
C63.11 F100.
Z-.3466
X2.435 F20.
G01 X2.192 F4.5
G42 C60.703 Z-.3007 F12.0
C60.567 Z-.2987
C60.409 Z-.2974
C60.24 Z-.297
C51.159 F14.2
C50.629 Z-.2979
C59.258 Z-.2987
C59.122 Z-.3007
C56.715 Z-.3466
G40
G00 X2.7
V1=36
VZSHC=VZSHC+V1
G00X3.0
G00 C0
RTS

[tarik1903]

Hello
You can do it by offsetting the tool from the machine panel.

[kurmay]

If you know how to use macro on okuma control, best way is writing a macro for C-Z offset

For example
V1=0.3 or V1=-0.15 (offset value)

For Z value we must write
Z[-0.3007+V1] or Z[-0.3007-V1]
Plus or minus sign is related direction

For C value
We need circumference of part diameter
V2=V1*360/[2.192*3.14/25.4]
C[60.703+V2] or C[60.703-V2]

[deadlykitten]

hello Lizz do you still need help ?

CZ compensation, for tool axis paralel to X axis, involves :
... g119
... if arches are needed : g132 133
... g40 41 42 obvious
... handling in-out compensation vectors, to avoid full C axis spin, as to avoid colisions on asimetrical shapes
... primitive diameter, in respect to section width
... tool offset shift, as the toolpath may not be designed on tool tip, but closer to the collet
... feed calculation, as CZ codes have different feed values, in respect to each axis; for example, feed for C only <> Z only <> CZ combos
... posibility to apply:
...... toolpath overall corections, especialy on non Y lathes, because toolholder may be offset in Y, not much, but > alowed tolerance
...... toolpath discrete corections, in geometry, depending on shape complexity
... HiCut for those small segments

a good postprocessor should handle all those

is not that okuma is complicated, but they allow adresing each atribute of milling with linear and rotary axis; as for next step, you can use inverse-time feed, as on 5 axis

please feel free to ask anything i can help you / kindly