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:

Dealing with "Potential C-Axis Instability"


Recommended Posts

So, I understand what the error is, but I can't find anyway to program it out. Multi-surface doesn't seem to have any way to define an approach angle.

How do you deal with this in mastercam? Seriously, how does mastercam not know where to start? the first line of the toolpath has a "B" and a "C" output, maybe it should start there?!?

J

Link to comment
Share on other sites

This is telling you that your Tool Vectors are almost vertical. When your tool path vectors become aligned with the "C-Axis", it will cause the C-Axis to spin, because "any C angle" is valid for a vertical tool Vector.

How do you stop it? Redesign your fixture so that your tool path is "tipped over" a few degrees, and the cut doesn't go "vertical".

Link to comment
Share on other sites

Or rotate your part .010 Deg in an axis that you DO NOT have (i.e. if you have an A/C Machine; rotate B.010, or if you have a B/C nachine rotate the part in A .010 deg). Often times this will get rid of singularity.

 

HTH

Link to comment
Share on other sites

Thanks,

I particularly like the idea of tipping the fixtures.

However, the problem I was having is not an issue with the toolpath per se, it's only with the approach, and only when I use a certain lead in. The toolpath against the part is all good.

A tangential line lead in causes the machine to rapid to the start point at "C0 B0" rather than the proper vector. The path would then get near the part at B0C0 then spin like hell to get the correct vector. The "c axis instability" prompt while posting would simply affect the C output of the first approach move.

When I disabled the line lead in,  the tool approaches at the correct vector and all is well.

I just figured that mastercam would always look at the start vector and (unless told otherwise,)pre-set the table to the right spot.

At least I know what to look for and what to tweak to get "post n' run" programs.

J

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...