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:

Peck drilling cycles


Recommended Posts

Hello, I am starting to use Mastercam and I noticed that when I set a peck drilling cycle for multiple holes, the Post processor (Generic Fanuc) create a Gcode with the complete G73/G83 instructions for the first hole and the only the coordinates of the other holes. I would like to have the complete G73/G83 command for each hole, like that it is easier to resume the code from any line. Is it possible?

Link to comment
Share on other sites

depending of the the post you are using, there may be a switch to output all codes for each hole

the other way to do it would be to make each hole a separate toolpath in Mastercam, but that would

make a simple task, complicated and error prone

Link to comment
Share on other sites

Try going into this section of the post

pdrill_2$        #Canned Drill Cycle, additional points
      pdrlcommonb
      pcan1, pbld, n$, pxout, pyout, pzout, prdrlout, feed, strcantext, e$
      pcom_movea

and change it to this

pdrill_2$        #Canned Drill Cycle, additional points
      pdrlcommonb
      pcan1, pbld, n$, pfxout, pfyout, pzout, prdrlout, feed, strcantext, e$
      pcom_movea

Link to comment
Share on other sites

You're i the wrong spot...gotta be...pfxout & pfyout are post blocks that force out the XY positions...unless someone has edited previously to remove it, something isn't right..

 

and this is out of the post you shared..

pfxout          #Force X axis output
      if absinc$ = zero, *xabs, !xinc
      else, *xinc, !xabs

pfyout          #Force Y axis output
      if absinc$ = zero, *yabs, !yinc
      else, *yinc, !yabs

 

So the post blocks are doing what they're supposed to...make sure you're editing the proper post....I've seen it too many times where someone is editing a different post then they "think" they are..

But changing those pxout & pyout to pfxout & pfyout should 100% get it

3N0QiNT.png

 

 

Link to comment
Share on other sites

Maybe I have not been clear enough in my first post... when I peckdrill multiple holes, I get a Gcode like this one:

N3756 G98 G83 Z-40.523 R-27.57 Q3. F160.
N3757 X0. Y29.3
N3758 X-25.375 Y-14.65
N3759 G80

 

Instead I would like to have this:

N3756 G98 G83 Z-40.523 R-27.57 Q3. F160.
N3757 X0. Y29.3

N3756 G98 G83 Z-40.523 R-27.57 Q3. F160.
N3758 X-25.375 Y-14.65

N3756 G98 G83 Z-40.523 R-27.57 Q3. F160.
N3759 G80

 

As you see, I get anyway the correct x,y for each hole, but I would like to have also the full gcode "G98 G83 Z... R... Q... F..."

Link to comment
Share on other sites

OK, so I went at this a bit differently to maintain the absolute/incremental flexibily...

I tested it quickly but don't fly blind with this until you've verified its accuracy across different uses.

TYa0woc.jpg

 

N100 G20
N110 G0 G17 G40 G49 G80 G90
N120 T124 M6
N130 G0 G90 G54 X-.0052 Y1.0964 A0. S1069 M3
N140 G43 H124 Z1.
N150 G98 G83 Z-.5 R.1 Q.125 F4.28
N160 G98 G83 X1.0208 Y.1432 Z-.5 R.1 F4.28
N170 G98 G83 X.9948 Y-.7526 Z-.5 R.1 F4.28
N180 G98 G83 X-.125 Y-1.3307 Z-.5 R.1 F4.28
N190 G98 G83 X-1.1823 Y-.5964 Z-.5 R.1 F4.28
N200 G98 G83 X-1.2344 Y.4505 Z-.5 R.1 F4.28
N210 G80
N220 M5
N230 G91 G28 Z0.
N240 G28 X0. Y0. A0.
N250 M30

 

**Edit, quick screen cap change, I had left out the peck1$ by accident

  • Like 1
Link to comment
Share on other sites
34 minutes ago, Zorander said:

you should edit "prdrlout"  ,  "refht_a " change  " *refht_a ". 

I disagree...

That will change it for all drill cycles...he has asked especially about peck drilling, that's exactly why I broke it out into the ppeck_2$  postblock

  • Like 1
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...