Work offsets changing

[swanny]

I have a few toolpaths with G54 and a few with G55. I have the planes set to a G55. I also go into my operations manager and set them there as well. When I post them together, G54 and G55, all toolpaths post as G54. When posted separately, they post correctly with the designated offset. No idea why. Generic haas 5 axis trunnion post, Mastercam X9.

[Reko]

Did you use -1 or 0 in your planes manager for G54?

 

Any way you can post the Mastercam file?

[Guest]

Go into your post and look for this

use_frst_wcs : yes$  #Use only the first WCS read and ignore all others in NCI

You'll want to set that for no

 

Personally, when I program for 5 axis, I prefer the 1 offset unless for some strange reason I really, really need another but if your setup is good, 1 offset should be fine 

[swanny]

Go into your post and look for this

use_frst_wcs : yes$  #Use only the first WCS read and ignore all others in NCI

You'll want to set that for no

 

Personally, when I program for 5 axis, I prefer the 1 offset unless for some strange reason I really, really need another but if your setup is good, 1 offset should be fine 

Thanks. I will look for that. If I was running one part like this I wouldn't bother with multiple offsets. But its easier to control during a run of 100 parts or so.

[Colin Gilchrist]

Are you using MPMaster? There is a Miscellaneous Integer that can be set for "locking" on the first work offset.

[gcode]

Are you using MPMaster? There is a Miscellaneous Integer that can be set for "locking" on the first work offset.

This is the mpgen 5axis post

[Rocketmachinist]

Has anyone tried modifying the post so you could use the actual offset you are looking for. Ie using a Zero or 54 , 1 or 55 , 2 or 56 and so on.

 

Sent from my SM-G930T using Tapatalk

 

 

[crazy^millman]

Put up the pwcs section of your post. I am thinking someone hard coded something in there.

 

HTH

[Colin Gilchrist]

Has anyone tried modifying the post so you could use the actual offset you are looking for. Ie using a Zero or 54 , 1 or 55 , 2 or 56 and so on.

 

Sent from my SM-G930T using Tapatalk

Yes, I do this for many of my clients. The only issue is if you have a shop with mixed controllers. For example, Okuma and Fanuc, and you want the flexibility to just change posts "on the fly". Okuma uses G15 H1, H2, H3, ect.

 

It works great on Fanuc based controls, with the the basic and standard extended work offsets G54.1 P1-P48. That way you can still enter "54" for G54, without interference. It gets trickier if you have P1-P100, or P300. For those cases, I usually try and convince people to just stick with the extended work offsets, or get creative.

 

For example, P1-P300, and enter '954' for G54, '955' for G55, ect. Then just add some logic in the post to subtract '900' from the value, if it is above 900. Otherwise you have to do something like use a Miscellaneous Integer, and it's just one more setting you have to remember.