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:

Toolpath Group Not showing in MPMaster Post


Recommended Posts

I need help with my modified MPMaster post the Tool path Group Not showing in option in Files Output comment.

Can anybody help me solving this problem?

Thanks.

 

 

Do you have the appropriate boxes checked in your control def. under nc output ? Did you go thru machine def. not just control def.? Dosen't stick unless I go thru machine def.

Link to comment
Share on other sites

Interestingly enough I'm not 100% sure that it is possible to output the toolpath group name. The control definition settings allow for the output of the machine name and the machine group name, but not the toolpath group name. Searching the nci parameter reference it looks like the parameter that was used for this was stripped out in X3, so I'm not sure that it is possible at this point... :blink:

Link to comment
Share on other sites

Do you have the appropriate boxes checked in your control def. under nc output ? Did you go thru machine def. not just control def.? Dosen't stick unless I go thru machine def.

 

 

I Sign all the boxes but Tool group info doesn’t work. Only Machine def, or Machine group but mostly I need Tool path group were I input OP number and description of operation.

Link to comment
Share on other sites

My apologies, 20018 is the parameter, not sure why it wasn't coming out in the other post I was using. This is what happens when you lose touch :)

 

So to answer the question just add this code into the pparameter$ post block

 

          if prmcode$ = 20018, stpgrpname = ucase(sparameter$)

 

Then output stpgrpname where ever you want the tool path group name output, likely ptlchg$, ptlchg_com or ptlchg0$

Link to comment
Share on other sites

This is in the post i am wondering if any of you can debuget and make it work.

thanks guys.

 

 

rd_mch_ent_no$ = syncaxis$ #Retrieve machine parameters based on current axis combination - read from .nci G950 line

rd_md$ #Read machine definition parameters - calls pmachineinfo$

rd_tlpathgrp$ # Read toolpath group parameters - calls pmachineinfo$

 

 

 

#if stpgrpname <> snull, pbld, n$, pspc, scomm_str, "TOOLPATH GROUP - ", stpgrpname, scomm_end, e$

 

 

[

if opcode$ = 13 & hst_flg, n$, pspc, scomm_str, "TOOLPATH - ", *sopnotehst, scomm_end, e$

else, n$, pspc, scomm_str, "TOOLPATH - ", *stoper, scomm_end, e$

if tool_op$ = 132,

[

Link to comment
Share on other sites

Looks like the post is already setup to handle the toolpath group comments.

 

Just take the # symbol away from the front of this line:

 

#if stpgrpname <> snull, pbld, n$, pspc, scomm_str, "TOOLPATH GROUP - ", stpgrpname, scomm_end, e$

 

Becomes:

 

if stpgrpname <> snull, pbld, n$, pspc, scomm_str, "TOOLPATH GROUP - ", stpgrpname, scomm_end, e$

Link to comment
Share on other sites
  • 1 year 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...