Sign in to follow this  
mats_asson

Add G0 first line after G41

Recommended Posts

In Traub TX8i systems you need to have a G0 line after starting a tool offset with G41 or G42.  Any idea how I could get a post to handle  this situation? I have a home made post for an Index machine that I just started to modify to suit our Traub machines.

Share this post


Link to post
Share on other sites

What is your base post?

Share this post


Link to post
Share on other sites

I don't remember what my base post was. I started the Index post when we had Mastercam version 8 or 9 something so it is ages ago. Probably one of the MPLFan posts that were available at that time. The offset is inserted in a psscomp postblock.

Share this post


Link to post
Share on other sites

That sounds dangerous. I would probably use stock to leave in that case.

Share this post


Link to post
Share on other sites

I know it sounds dangerous but that is the way Traub have done it. There is no movement in the G0 line. It just somehow tell the machine how to position for the next cut. And you also need to use "control" compensation instead of "wear" that I normally use. Traub has it's own special way of treating G41 and G42. They also have G46 for turning which handles offset without needing to tell which side you turn on. That information is fetched from the tool quadrant setting.

Share this post


Link to post
Share on other sites

What does the actual code end up looking like? Is there still a G1 in the call-up, then a new line with just G0 on it?

Share this post


Link to post
Share on other sites

im by no means a postmaster but if you could post code of how you want it to be, would help a lot.

Share this post


Link to post
Share on other sites

Finally I remembered to get some code from work!

This is roughly the way I get it from Mastercam and the way that seems "normal" for most machine types:

G0 X27.569 Y18.13 Z2.
G1 Z-6.5 F250.
G41 X23.6025 Y16.005
X23.8385 Y15.565
 

and this is the way that the Traub machines wants it to be. I have no idea how the control system designers 
heads are working. The G0 after G41 is not a rapid move. It just needs to be there. I also need to have 
control compensation type instead of wear. Do you think this is strange? Me too.. but it is the way it is.

G0 X27.569 Y18.13 Z2.
G1 Z-6.5 F250
G41
G0 X23.6025 Y16.005
G1X23.8385 Y15.565
 

Basically, what I need, is a way to find out if the G41 is being posted so I can post out the G0 the way I want.
If I remember correctly I have tried to check if cc_pos$ = prv_cc_pos$ but it didn't work. It is a while ago so 
I don't remember the details.

     Best regards, Mats

Share this post


Link to post
Share on other sites
plinout         #Output to NC of linear movement - feed

       if cc_pos$ <> prv_cc_pos$ & cc_pos$ <> zero,
	   [pccdia, e$
	   pcan1, pbld, sgfeed, sgplane, "G0", sgabsinc, pwcs, 
        pxout, pyout, pzout, pcout, strcantext, pscool, e$]
     else,[
       pcan1, pbld, sgfeed, sgplane, *sgcode, sgabsinc, pwcs, pccdia,
        pxout, pyout, pzout, pcout, feed, strcantext, pscool, e$]

This got it outputting mostly what you want, changing the `sgcode to *sgcode forces it to output G1/G0 every line tho, without changing it, bad things happened.

Share this post


Link to post
Share on other sites

Create an account or sign in to comment

You need to be a member in order to leave a comment

Create an account

Sign up for a new account in our community. It's easy!

Register a new account

Sign in

Already have an account? Sign in here.

Sign In Now
Sign in to follow this  

  • Recently Browsing   0 members

    No registered users viewing this page.

Join us!

eMastercam - your online source for all things Mastercam.

Together, we are the strongest Mastercam community on the web with over 56,000 members, and our online store offers a wide selection of training materials for all applications and skill levels.

Follow us