My sweep won't regenerate

paul_1 · January 2021

I'm trying to sweep a profile along one quarter of an elliptical path. The error is that "Result of sweep intersects itself", but I'm not seeing how that's possible, and the picture Onshape shows me isn't helping. I can't help but think I'm making a beginner mistake... because that's exactly what I am. ;-)

paul

https://cad.onshape.com/documents/71bc7524278347a0ac933851/w/e253e8b86328f1385d062732/e/7f1c0dc00108acc413ca5c73

wayne_sauder · January 2021

Then you could use a surface to split and delete. I not sure that is the best way but it would work. See example.https://cad.onshape.com/documents/b0abedc6843cf229ab4f8fac/w/99c7f636901fd0928c97cbb3/e/10de34ce674fa223c1fc3ab8

Prachi · January 2021

An other thought starting with a swept surface and adding fills. The last fill closes the surface and makes a solid.
https://cad.onshape.com/documents/2d9bc9b86baef5743483a868/w/6ed23a39392f04ecf5486cf8/e/a378c42a0636c0dc798d70b6

wayne_sauder · January 2021

You got the idea, after looking at this a bit closer, I realize the real issue is that a sweep produces self-intersecting geometry, that is the reason it is failing not because of the collision with the existing part. Here is another way of doing what you want with fewer steps. https://cad.onshape.com/documents/b0abedc6843cf229ab4f8fac/w/99c7f636901fd0928c97cbb3/e/079e07e839ecd2d998df5827

Image: https://us.v-cdn.net/5022071/uploads/editor/rm/j28e7aizixty.png

wayne_sauder · January 2021

I would use the revolve command for that. https://cad.onshape.com/documents/b0abedc6843cf229ab4f8fac/w/99c7f636901fd0928c97cbb3/e/10de34ce674fa223c1fc3ab8

wayne_sauder · January 2021

If you only want a surface you could use a sweep. I'm not sure what your design goal is, see the copy that I made. I changed your sweep to a surface and also did a revolve.

paul_1 · January 2021

Thanks! I wish I could do a revolve, but I can't because the path is elliptical. And yours is circular. (Mine was very close to circular -- I've changed it to make the shape more obvious.) My design goal is some much like you produced, but based on an ellipse (or, maybe even, a spline).

wayne_sauder · January 2021

Then you could use a surface to split and delete. I not sure that is the best way but it would work. See example.https://cad.onshape.com/documents/b0abedc6843cf229ab4f8fac/w/99c7f636901fd0928c97cbb3/e/10de34ce674fa223c1fc3ab8

wayne_sauder · January 2021

The sweep as you are using it

Image: https://us.v-cdn.net/5022071/uploads/editor/ph/gsrww6mgsxn1.png

is trying to cut through your existing part.

wayne_sauder · January 2021

I made a correction in my example.

paul_1 · January 2021

wayne_sauder said:

The sweep as you are using it is trying to cut through your existing part.

Yes, I saw that -- but that little "tang" only appeared after I changed my example. And it's not at all clear where that little thing is coming from.

paul_1 · January 2021

So, if I understand what you did: You used the same sweep I did, but didn't include the lower rectangular sections, in order to just create a surface. (I didn't know that was possible, so this is good.) And then you encapsulated it in a revolve, though it could have been any shape, right? Like a rectangular block? And then you used the surface created with the sweep to split the new solid, and then deleted the part you didn't want.

Okay, I can do that. I'm curious as to why what I did didn't work, but I'm happy with a workaround.

Thanks!

Prachi · January 2021

An other thought starting with a swept surface and adding fills. The last fill closes the surface and makes a solid.
https://cad.onshape.com/documents/2d9bc9b86baef5743483a868/w/6ed23a39392f04ecf5486cf8/e/a378c42a0636c0dc798d70b6

wayne_sauder · January 2021

You got the idea, after looking at this a bit closer, I realize the real issue is that a sweep produces self-intersecting geometry, that is the reason it is failing not because of the collision with the existing part. Here is another way of doing what you want with fewer steps. https://cad.onshape.com/documents/b0abedc6843cf229ab4f8fac/w/99c7f636901fd0928c97cbb3/e/079e07e839ecd2d998df5827

Prachi · January 2021

nice step reduction.

paul_1 · January 2021

glen_dewsbury said:

An other thought starting with a swept surface and adding fills. The last fill closes the surface and makes a solid.
https://cad.onshape.com/documents/2d9bc9b86baef5743483a868/w/6ed23a39392f04ecf5486cf8/e/a378c42a0636c0dc798d70b6

Wow -- I never would have thought of that technique. I'm surprised it's possible to define a fill that doesn't actually describe a volume! But just by describing several surfaces (planar or not) as fills, the volume they enclose becomes solid. Slick.

romeograham · January 2021

The technique you guys arrived at (sweeping a profile that doesn't fully-define your finished shape) then using other tools to create the final shape is (I think) the best approach.

Another robust tool for creating the solid in after you have the swept surface (or solid) is the Enclose command. It's under the Thicken command.

Enclose is handy because you can use planes as inputs...this means that you can use your cardinal (or other) planes, and avoid creating extra features or geometry.

My sweep won't regenerate

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