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:

multiaxis toolpaths locked to 3 axis on HMC?


motor-vater
 Share

Recommended Posts

Can anyone help me make sense of how the planes affect this. Lately I am using more of the multiaxis stuff locked in 3 axis. But on horizontals this gets tricky. I use Top, Front, Front always and usally program from center of rotation with as many incremental values as possible. Some of these tool paths work great others get completly out of control because of the multiple plane selection windows. Its driving me crazy. I hate using suface contour anymore, and love the roughing and undercutting abilities of Triangle mesh and multi-parallel but dam it if its not a chore every time to get them to work on a hori.. Any help or guidance is appreciated.

Link to comment
Share on other sites

Been A while if I check to see if they have become Plane aware. I got always from using the Clearance planes for the retract and clearance and just use the rapid planes. Set those values to amounts I need and done. Don't forgot point toolpaths they help a lot. You have ref points, but they have to be manually done and how they work in other parts of the software is night and day different.

Link to comment
Share on other sites

Right.  Remember that any reference to an axis (X,Y,Z) in a multiaxis toolpath is relative to the WCS of that toolpath (in your case, TOP), to elaborate on why Mayday is correct.  The "Front, Front" part of your plane selection really has no bearing on anything here. 

In the case of your clearance plane when you're programming Top, Front, Front, you're retracting along the Y relative to the Top WCS, NOT the Z.  If you were on the Top, Back, Back, you may need to retract -Y, for example.  Right & Left would be along the X.

  • Thanks 1
Link to comment
Share on other sites

Ill give it a go and see what happens.. lol but to be clear I am staying on Top, Front, Front and then retracting on Y.  I feel like I have tried this before but Ill try to paint my self into a corner again in the morning.. I seem to have the least amount of problems with parallel. I have made that work a few times but seems like Triangle mesh, constant Z is one of the ones I struggle with. It sounds like the toolpath I want to use alot of times cause of the ability to make it spiral/ramp down in things like pockets. But Im working off memory for the moment I'll play with it a bit in the morning and pinpoint the area of confusion. A part I am working on at the moment would benefit greatly from these tool paths. They never give me the easy stuff anymore... errr

Link to comment
Share on other sites

In general, Parallel will often give a better toolpath than Triangular Mesh, just based on the underlying technology.  The equivalent of "constant Z" is to use Parallel set to "Angle" (as in, "the path will be parallel this angle").  Of course, you can always convert it into a spiral instead of an actual constant z, water-line style toolpath just like you can with Triangular Mesh. 

  • Thanks 1
Link to comment
Share on other sites

Aaron thanks a million my friend. I made some pretty good progress with these toolpaths today. Got a few ops to work the way I wanted them too, and discovered the hidden gem (project curve) worked wonderfully, way better with check surfaces and lead in/out than any of the conventional tool paths.

A few of the other things I attempted are still problematic, seems like controlling over all cut depths( mainly start depth) is not happy as well as undercuts (allready unchecked extend toolholder to infinity), I can make them work for a vertical, but in a horizontal environment. Some more experimentation is in order. I feel like these paths offer so much more than the old stuff and best of all they dont take 10 min to regenerate like surface finish contour can.

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...