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 am trying to use Curve to corner round as much of this part in one smooth motion. the tool is transitioning too slowly around the 90 degree corners. Sadly my shop only has curve so it's my only option. Does anyone have advice on how to get the transition to happen 100% on the corner? I added extra tool axis control lines but it still doesn't orient correctly until it gets to the middle.

image.thumb.png.307c7c9c40d23e8009f7f934fe1b4479.png

Link to comment
Share on other sites
7 minutes ago, cncappsjames said:

You could do it that way but where's the fun and growth in that? :D

Well I suppose there isn't much there.... sometimes less is more...and it would run faster and blend like a dream... as far as acceleration around corners we working with  Siemens or Fanuc controlled machine if its a Siemens get that cycle 832 loosened up and let er rip....

Link to comment
Share on other sites
7 minutes ago, cncappsjames said:

Often times when doing edge treatments I do a full 5-Axis path in order to maintain consistency because I can keep the tool in contact with the part at all times. Excessive? Maybe. Then again maybe not. It all depends. 

It's a more efficient path so it's faster, less cost to the customer and keeps your skill sharp.

Excessive, I think not.

Link to comment
Share on other sites
26 minutes ago, Bbeyer562 said:

Well then on your cut pattern page there should be a box that says maximum step choke that down smaller and see if it helps ya out

This maximum step is used to output more or less vectors. But you don't need more Vectors in the straight sections. Instead, go to the Tool Axis Control page, and use the 'angle' function to force out more Vectors in areas with actual 'rotation'. I typically use 0.5 degrees, 0.2 degrees, or 0.1 degrees. Sometimes I have to drop it down to 0.01 degrees...

  • Like 1
Link to comment
Share on other sites

I forgot about that setting too..... The Grob 5 axis machines I program  seem to love all the vectors you can feed them so I usually pile em on heavy and then dial my cycle 832 settings with a decent angle tolerance and let it chow down like pac man. 

  • Like 1
Link to comment
Share on other sites

If all you are doing is the radius on the edges, you could do it with a "simple" 3 axis toolpath.  Morph between 2 curves is effective at this, even with only 3 axis moves.  

Under "Cut Pattern", set "Pattern From" and "Pattern To" as edge curves on your model (on each side of the radius), select the radius as the drive.  Under "Collision Control" #2, set check surfaces as your wall geometry.  Under "Additional Collision Control Strategy", set #3 check surfaces as your floor geometry.

Here is a MC2020  example of one that the radius goes all around and up & down the walls. The radii in the corners are mitered in this case, which is tougher than gliding down a radius through the corner.

 

Morph between 2 curves.mcam-operations

Morph.JPG

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...