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:

lathe c axis contour


Rocketmachinist
 Share

Recommended Posts

  • 5 months later...

Ok cool I finally got 5 axis added onto my lathe mill hasp. The downside is when I select a 5 axis toolpath to try to do this part a different way I get the error message (incorrect axis combination) . What kind of stuff do I need to add to the machine definition to let me load 5 axis toolpaths but not mess up my post.

 

The lathe is an old Haas SL-20 without a y axis but with live tooling.

Link to comment
Share on other sites

Go into the Machine Definition Manager, and find the branch in the Kinematic Tree, that ends with your Turret Component. Add two Rotary Components in-between the linear components (X, or Z, depending on how the MD was originally built).

Example:

-Lathe X Linear

     -Lathe Z Linear

          - Lathe A Axis

              -Lathe B Axis

                 - Lathe Turret

Then, go into your Axis Combinations dialog box (button on the top row), and edit the existing Axis Combination. (Uncheck the Turret, then check the two rotaries, and then check the Turret). This adds the two rotaries to your Axis Combination.

Another option that sometimes works is to simply create a 2nd Axis Combination. Have the 1st Axis Combo be set to X Z C, and the 2nd combo set to X Z C A B. By just having the extra Axis Combination available in the Machine Definition, this can be enough to fool some of the tool paths into letting you use them.

The Mastercam Tool Paths have some logic built into them to check and make sure that the Axis Combination would support a full 5X path, even though you'll be restricting the actual output to a single rotary, and locking the tool axis so it is perpendicular to the Spindle Centerline. So this "trick" is really more about faking out the Mastercam interface internal "safety check". It "shouldn't" affect the output of your post, but is also depends on when your post was built. There is some logic in modern posts to check and see if there are more than 1 rotary axis components present in the Axis Combination, and if true, then the Post will throw and error and stop processing. If that is the case, I can help you edit the post to eliminate the error.

Basically, Mastercam is attempting to "save you from yourself", by restricting the tool paths you can run, based on the capabilities of your specific machine. This also comes into play when you are doing a "replace" on the Machine Definition. Mastercam will scan through your existing tool paths, to see if they are "compatible" with the machine you are trying to use. If you don't have the same rotary configuration, Mastercam throws an error and won't let you replace the machine.

For Mastercam Mill, this is the reason that the "Default" Machine Definition (tied to MPFAN), has 3 rotary components: A, B, C. By having all three rotaries present in the MD, it tells Mastercam that "this machine could potentially achieve any rotary combination (A/B, A/C, B/C), so allow this machine to replace any existing Mill...

-------------------

To "unwrap" geometry, use the Xform - Unroll command.

Link to comment
Share on other sites

I did also figure out recently how to use c axis contour. The most important part of the whole thing is the rotary axis control- rotary diameter. It should be set the the diameter of the geometry you selected. Then the depth of cut is pretty much incremental even though its claimed to be absolute.

unroll%20tolerance_zpsuol30ppg.png

linking%20parameters_zpszusztcus.png

backplot_zpssyzhaiob.png

geometry_zpsq6sii0ol.png

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...