G53 posting instead of G54

[NATE]

We have been running Ver.8 and just loaded Ver.9, I updated the posts and everything works good except it gives a G53 code instead of G54 like before. I know this has to be a simple fix, I just can not seem to find it. Thanks in advance for the replies.

[deanj]

Nate, I recently had this same problem with V8 except I wanted to change my G54 to a G55. I'm assuming v8 and v9 are similar in this manner so here it goes. You may need to change two settings depending on how your post is set up. In MC go to toolpaths-

operations-

perameters-

TCplane-

check toolplane box-

go to work offsets box, 1=G54 2=G55 and so on...

(at least on my comp)-

run a couple of posts with different settings see if that works.

 

If not go into your .pst file scroll down to the

--------------------------------------------

default miscellaneous integer values

--------------------------------------------

go to default work coordinate systems and switch accordingly.

 

I had to screw with these settings a couple times to get it right but eventually it worked.

 

Hope this helps, JMD

 

[ 07-10-2002, 04:06 PM: Message edited by: deanj ]

[Greg Williams]

Nate,

 

Personally I think that 1=G54 2=G55 so on is a pain in the butt I prefer the second option of 54=G54 55=G55 and so on I find this much easier. The only problem is that you need to edit your post to look like this

 

pwcs #G53+ coordinate setting at toolchange

if mi1 > one,

[

sav_frc_wcs = force_wcs

if sub_level, force_wcs = zero

if workofs <> prv_workofs | (force_wcs & toolchng),

[

if workofs > 53,

[

g_wcs = workofs # + 53

*g_wcs

]

else,

[

g_wcs = 54

*g_wcs

]

]

force_wcs = sav_frc_wcs

!workofs

]

 

You will notice that this post will not output G54.1 which is how I want it as I never use G54.1

[Jim Evans from CNC Software]

Nate,

 

First edit your post and search for the variable WORKOFS. If you find this variable in your post, check to see if there is a formula related to it (g_wcs = workofs + 54 this is from the MPFAN post). Next edit your NCI file and search for the 1016 NCI line and check the 9th parameter. If the 9th parameter is less than zero and your post is using the WORKOFS variable, then this is your problem and this is also a bug. Please report it to [email protected]. The 9th parameter should NEVER be anything less than zero.

 

If the 9th parameter is not less than zero, check your formula if you found one. If none of this helps, please contact your local Mastercam Reseller.

 

There have been bugs in the past where the 9th parameter of the 1016 NCI line was written out as -1 to the NCI, which would cause a G53 in all of our posts.

 

I hope this helps!

[NATE]

Jim,

My NCI does post out a -1. The funny thing is when I post from the operation manager it posts normal with a G54.

 

Thanks everyone for the help

[Jim Evans from CNC Software]

Nate,

 

This is a known bug, but I hjaven't checked to see if it was fixed yet.