Need help with OSAI post proceoor.

[notlukydog]

I am looking for a post processor for the CR Onsrud HD Series model 122HD18. I have been using mastecam and have the post processor for that software but all I have is the Generic OSAI from HSMwowrks. With the Generic post, I get incompatable Gcode and UAO offsets at the end of the toolpathing. The PP0002251.nc is the file that mastercam post and the 2 contuor.nc is the file that HSMworks posts out. I have the mastercam post file, if that would help at all. I also have a list of compatable gcode for the machine.

Any help would be appreciated.

Thank you

Kevin

[skidsolo]

This post processor is running at a furniture factory.

[notlukydog]

Thank you skidsolo,

I was able to use the post with a few mods.

I had to delete

N3 ; ACTIVATE G500 FILTERING MACRO
N4 G500 T20 F32

The multi axis uses A, B, C

I had to also delete all the,

N14 G0 A0. C0.

and

N17 (UIO,Z(-1*L370))
N18 (TCP,5)

The rapid code showed in the setup and right after the tool change. The other code showed after tool changes and end of toolpaths.

I have no idea what G500 is.

I was able to modify the post to get ride of the G500, UIO and TCP lines. But I was unable to figer out the rapid with A and C axis. I removed it in the setup by changing it to X0. Y0. but it still shows up after the tool change. Would you have any idea how to remove it?

Again, thank you so much.

Kevin

[skidsolo]

UIO,Z is use incremental offset from work origin, TCP,5 is used to retract the tool on a virtual axis with the heads tilted.

the other G0 A0 C0 comes from this code in the post:

if (insertToolCall) {
gMotionModal.reset();
setWorkPlane(new Vector(0, 0, 0)); // reset working plane
forceWorkPlane();