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:

Recommended Posts

I've noticed issues when I transform toolpaths and use incremental...  I think it's a post issue, which is why I am seeking help here.  The issue is, when I transform translate a toolpath and use incremental to reduce program size, if I have a rotation, it will still be in incremental during the rotation and won't go back to absolute until the next X axis or Y axis motion.  I've had this bite me several times and was wondering if there's a way to make it go back to absolute on the A axis motion as well?  Maybe have it end subroutines with a G90 or something.  Any ideas???  Thanks!

Link to comment
Share on other sites

Sample code and step by step screen shots or word doc showing your steps. Without more information or detail I and I suspect many others will be throwing dart at the dart board in the dark blind folded. A .z2g with your post and sample file will be helpful also.

MLC CAD your dealer should be able to help have you reached out to them?

Link to comment
Share on other sites

For a real quick fix, just put a

G0 G90 A270 

That will fix the "now" problem

You could edit this line as I have done

ppos_cax_lin    #Position the rotary axis before move - rapid
      if index, pindex
      else,
        [
        if fmtrnd(prv_cabs) <> fmtrnd(cabs) & rot_on_x,
          [
          sav_gcode = gcode$
          gcode$ = zero
          if convert_rpd$, pconvert_rpd
          pbld, n$, [if gcode$, sgfeed], *sgcode, *sgabsinc, pcout, [if gcode$, feed], e$  <<<<<<<This Line
          !cia
          ps_cinc_calc
          gcode$ = sav_gcode
          ]
        ]

N450 M98 P0001
( RAMP CONTOUR 3 X 17 X THRU OBROUND )
( G59 90 DEG )
N460 G0 G90 A-270.    <<<<See the change
N470 X5.3843 Y.2034
N480 M98 P0002
( RAMP CONTOUR 3 X 17 X THRU OBROUND )
( G59 90 DEG )
N490 G90 X6.3686 Y.2034
N500 M98 P0002

Edited by Guest
Link to comment
Share on other sites

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...