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sweep 3d fit spline

hervé_piponhervé_pipon Member Posts: 60 ✭✭
Hello
I want to sweep a circle along a 3D fit spline...
The part stays red but I dont know why it doesn't work  
Can you give me some clues
https://cad.onshape.com/documents/e8d2062de0ff95f77a6b4b37/w/88f7579ccec47391700eef0d/e/11c1c545df40cf3e4129269f?renderMode=0&uiState=62166a218a7f740bc888c9bb

Best Answers

Answers

  • imants_smidchensimants_smidchens Member Posts: 62 EDU
    Answer ✓
    as far as I can tell, the issue is that "Sweep 2" creates a self-intersecting part at one end. Zooming in reveals the problematic geometry with the curve with the sweep profile running into itself.

    this can be solved by adjusting the start magnitude in your 3D fit spline from -0.037 to at least -0.051 (anything larger will also work)
  • GregBrownGregBrown Member, Onshape Employees Posts: 93
    Answer ✓
    Hello
    I want to sweep a circle along a 3D fit spline...
    The part stays red but I dont know why it doesn't work  
    Can you give me some clues
    https://cad.onshape.com/documents/e8d2062de0ff95f77a6b4b37/w/88f7579ccec47391700eef0d/e/11c1c545df40cf3e4129269f?renderMode=0&uiState=62166a218a7f740bc888c9bb
    It looks like a combination of the 1) diameter of the sweep profile (in Sketch 9) is too big, and 2) the curvature (Start Magnitude) in 3D Fit Spline 1 is too low. I can get it to regenerate with some tweaking...
  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 2,005 PRO
    edited March 2022
    This issue has been around for awhile. I found this to be true with the cable FS I wrote a couple of years back and is the main reason I haven't released it into the wild.



    When I asked for the end of the sweep to be normal to the face, if became extremely unstable and I chose to turn the norm constraint off. 

    My solution, which I haven't done yet was to trim/move/boolean the sweep to the face making this operation into 2 features vs. just a sweep. I didn't test this solution for robustness and need to. 
  • billy2billy2 Member, OS Professional, Mentor, Developers, User Group Leader Posts: 2,005 PRO
    edited March 2022
    From the user interface, I've tried:

    boolean subtract:

    This is what I'd do. It seems to be the cleanest and will be my solution when I get some time to implement.


    split part:

    Split worked but you'd have to follow up with a delete body and figure out which body to delete.



    move face:

    This doesn't work very well.


    This means you could rewrite the sweep feature and call it robust sweep to handle the end condition. Have you tried feature script?


  • Evan_ReeseEvan_Reese Member Posts: 2,056 PRO
    I think you've already got this solved, but for future diagnosis you can also right click the curve (or right click in space while you're editing the fit spline feature) and select "Minimum radius" to see the tightest curvature on the curve. If your tube radius is bigger than the minimum, it will self-intersect and fail. I think in your case you curve looked smooth to the eye, but was actually slightly hooked at the end. I made a gif below to show what that might look like, and how to tell.

    Evan Reese / Principal and Industrial Designer with Ovyl
    Website: ovyl.io
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