Jump to content

Welcome to eMastercam

Register now to participate in the forums, access the download area, buy Mastercam training materials, post processors and more. This message will be removed once you have signed in.

Use your display name or email address to sign in:

Generic Haas VF-TR_Series 5X Mill post


MSL
 Share

Recommended Posts

Hi,
I noticed on new Generic Haas VF-TR_Series 5X Mill post we have an option to switch to G28 or G53 home.
But none of these options sends the machine's Y axis home at the end of program. What would be the best approach to send the Y axis home only at end of the program?

Thank you.
Link to comment
Share on other sites

John is right. You can code this move into the "peof$" Post Block.

Typically, the first line in 'peof$' makes a call to 'pretract'.

Inside of 'pretract', you have this logic:

      if nextop$ = 1003 | tlchg_home, pbld, n$, *sg28ref, "X0.", "Y0.", protretinc, e$

The "if nextop$ = 1003" is used to flag "end-of-file". You should uncomment this line (if commented out), or add this line to your post. (May have to remove the 'tlchg_home' condition, if you don't have that switch in your Post.

Depending on how the logic is setup in the VF_TR Post, it may be using 'sg28ref' to output the "G53" command.

It might just be easier to add the line directly to 'peof$', after the call to 'pretract'...

  • Like 1
Link to comment
Share on other sites

Thank you John and Colin,

I added these lines after pretract in "peof" and It outputs the codes I wanted.

 pretract
	  
	  if return_mode = one,
        [
        #pbld, n$, *sgcode, *sg28, *sgabsinc, "Z0.", e$
	pbld, n$, *sgcode, *sg28, *sgabsinc, "Y0.", e$       
	]
	else,
        [
        #pbld, n$, sg53, *g53_return_z, e$
	pbld, n$, sg53, *g53_return_Y, e$                    
	]

 

  • Like 2
Link to comment
Share on other sites
  • 3 months later...

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.

 Share

  • 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

×
×
  • Create New...