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Yet another Loft question

tom_augertom_auger Member Posts: 134 ✭✭
in Community Support

Sigh. Lofts.

I deliberately built these three profiles to have the same number of points, and drew them in the same clockwise order, I'm even using Connections and yet the loft engine somehow is twisting two pairs of vertices.

How to disentangle this mess?

image.png
Tagged:

Answers

  • Kevin_CowlesKevin_Cowles Member, Onshape Employees Posts: 73 image

    Do you have a link to the model? It could be that its self intersecting regardless of having the correct connection points defined. Happy to peek!

  • S1monS1mon Member Posts: 4,187 PRO

    Can you share a public document? That doesn't look like something where you should need to manually use connections.

    Simon Gatrall | Product Development, Engineering, Design, Onshape | Ex- IDEO, PCH, Unagi, Carbon | LinkedIn

  • tom_augertom_auger Member Posts: 134 ✭✭

    Thanks @Kevin_Cowles and @S1mon for being generous with your time on this.

    Here's a shared link: https://cad.onshape.com/documents/d372e0f2c329dfb8015def94/w/a7eeda0f8870916fcf82d1ce/e/97b24175a4f9db2b41f41d68?renderMode=0&uiState=69cedd1265d0d166f12491c7

    I can make it "work" if I loft in two parts and boolean the whole thing.

    I was also surprised to learn that the guide edges must be coincident with the edge of any profile being used. For that reason, I would need to make a few adjustments to use the guide edges, but that was a step I was reserving after I got the loft to work on its own.

  • S1monS1mon Member Posts: 4,187 PRO

    That ended up being more complicated than I initially thought. A few issues:

    1. Some of your sketches were not fully defined. This can cause a lot of issues with loft profiles lining up with guides.
    2. Connections work when Loft can easily create some splines to connect the profiles, but in this case, it wants to make edges which twist over one another which is a no-go.
    3. It's not entirely clear what you were after, but I made some guesses.
    4. It's sometimes easier to model things as surfaces and then make a solid.
    5. I'm sure I could have taken fewer steps, but I leave that for you to clean up

    https://cad.onshape.com/documents/2a4e2ca3944301233394e733/w/7ce157ee9051f8a5f04dfd6b/e/c17914bd587f011b7649ea00

    image.png

    Simon Gatrall | Product Development, Engineering, Design, Onshape | Ex- IDEO, PCH, Unagi, Carbon | LinkedIn

  • tom_augertom_auger Member Posts: 134 ✭✭
    https://forum.onshape.com/discussion/comment/129065#Comment_129065

    Thanks for your help @S1mon ! I'll need some time to digest this different approach.

    Any guesses as to why the loft didn't work?

    In other software I have seen situations where the curves created by the splines that are created by the loft force a crossover, but in that case it should have happened to all the sides, not just a single edge, so I'm still confused. In those cases, the solution would be to have more intermediary profiles to force the splines to conform, so I'll try that here.

    The approach I ended up going forward with was to simply do the loft in two segments (top and bottom) and then union the two, which in this case worked out, but in other cases would have produced a sharp transition where one would have wanted a smooth one.

    Lofts continue to be my worst enemy. I really need to invest some time in learning surface modeling.

  • S1monS1mon Member Posts: 4,187 PRO

    When there’s an issue like that cross over, it only shows the first error. I would assume that it would create the same issue with the other side. I think you can verify this even lofting just that surface without the guides.

    Typically you don’t want to add lots of profiles because that will just make the loft surfaces that much more complex and potentially lumpy. Breaking things up and/or guides is likely a better option.

    Simon Gatrall | Product Development, Engineering, Design, Onshape | Ex- IDEO, PCH, Unagi, Carbon | LinkedIn

  • MDesignMDesign Member Posts: 1,381 PRO
    image.png

    Connections aren't going to help in this situation. Like Simon suggested the error is present on both sides. you can test that by making you mid profile thicker on one side to resolve the crossover that is happening as the result of the way OS has to flow the corners to each other. How to resolve it depends on your desired final geometry.

  • MDesignMDesign Member Posts: 1,381 PRO
    image.png

    You could do the base loft and set end conditions and then add the longer portion as another loft (no need to boolean) and set end conditions with magnitude control.

  • CADNurdCADNurd Member Posts: 145 ✭✭
    edited April 5

    Thought I might have a 'stab' at this one (pun intended)

    No surfaces or curves in my attempt - just solids.

    https://cad.onshape.com/documents/806b4b83757bb7dd2196819c/w/b5e8fdbd60c6cf633fe57257/e/800b951c9e0f5ceed08e0296?renderMode=0&uiState=69d2d6306cc4d1d1e493ccad

    Screenshot 2026-04-05 22.21.32.png

    Unemployed Onshaper - Operating on European time - More of me here ➤➤ https://linktr.ee/Liam.G

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