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:

Dynamic mill burying the tool


Sticky
 Share

Recommended Posts

It is a .5" tool, using a .1" RDOC and .05" min rad. The bottom slot width where the tool gets buried is .875" wide. The weird thing is that it does almost the entire slot width before it buries itself. WTF?

Yes is the reposition move with never it is moving over to the next place through the material, When you using the when exceeding a distance you will get a retract move, but it does not go through the material to get there where as never will do that. Again I just got away from using never and still back plot my tool paths and watch it move by move. Once they put in volumatic checking into the algorithm then this will hopefully be a thing of the past.

Link to comment
Share on other sites

Between the middle boss and the wall?

 

Backplot it and watch very carefully. It can be deceiving looking at the path only.

 

No, while that one doesn't look so great either it's not as bad the the area where the hole is, it's hard to see:

 

post-40824-0-52378700-1419892189_thumb.jpg

 

I'm working on a file to upload now.

Link to comment
Share on other sites

This is why I use optipath in vericut to monitor the volume removal rate, it can be set up to check for cuts like this even if you do not buy the optipath license.

 

Kevin C.

 

Kevin is right, he found this out about the tool path using vericut, it is the best way to keep mastercam honest - it constantly over engages, mostly in the entry arc - it affects tool life drasticly in hard metals because of this, the material removal rate is not consistant. This needs to be addressed.

Link to comment
Share on other sites

Ben K is correct - if you select a solid face with two holes (like this one) for your machining region, the path will extract three loops and machine all three independently.  In this case, unfortunately, the ordering is such that the two holes are machined first then the outer loop.

 

Ben's suggestion is on target- just select the outer loop as your machining region.

 

It works this way for solid faces and for wireframe area selection.  And it works this way, too, in X6 and X7 multiple region (not single region).

 

This is a good part to show the issue; I'll share it with my team to see if we can provide better assistance (a warning message or better machining order).

 

Thanks,

Bill B

Link to comment
Share on other sites

Ben K is correct - if you select a solid face with two holes (like this one) for your machining region, the path will extract three loops and machine all three independently.  In this case, unfortunately, the ordering is such that the two holes are machined first then the outer loop.

 

Ben's suggestion is on target- just select the outer loop as your machining region.

 

It works this way for solid faces and for wireframe area selection.  And it works this way, too, in X6 and X7 multiple region (not single region).

 

This is a good part to show the issue; I'll share it with my team to see if we can provide better assistance (a warning message or better machining order).

 

Thanks,

Bill B

 

 

Ahhh, that makes sense, I see that Ben mentioned it but it didn't click for me that it was picking the holes, but it makes perfect sense that it does.

Link to comment
Share on other sites

Ben K is correct - if you select a solid face with two holes (like this one) for your machining region, the path will extract three loops and machine all three independently.  In this case, unfortunately, the ordering is such that the two holes are machined first then the outer loop.

 

Ben's suggestion is on target- just select the outer loop as your machining region.

 

It works this way for solid faces and for wireframe area selection.  And it works this way, too, in X6 and X7 multiple region (not single region).

 

This is a good part to show the issue; I'll share it with my team to see if we can provide better assistance (a warning message or better machining order).

 

Thanks,

Bill B

 

This is a much better explanation than I provided. Thanks for expanding on the subject. :cheers:

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...