Is it possible to make a self-intersecting sweep?Who knows what tools can be used to do such work.

dmytro_semenov

MDesign

Do the sweep in sections that don't self intersect the section being created. and merge them together as you create them.

MichaelPascoe

Since this is a flat-ish part, you could just use the Extrude thin. Then add some fillets or chamfers to handle the edges.

dmytro_semenov

You saw the number 4. It intersects everywhere.

MichaelPascoe

This was quite a bit of a pain to get to work. Looks like extrude thin couldn't handle it. Neither could draft, or body draft, or sweep, or offsets, or move face, move boundary, ruled surface… Using a standard extrude, thicken, and fillet, seemed to do ok:
https://cad.onshape.com/documents/c04a35e0c62a01b4b0cd3847/w/930f07bb98ff6b72d69bb6f5/e/6...

Render studio also seems to have improved its intuitive-ness. Thanks Onshape team! 😎

MDesign

Thanks for the push @MichaelPascoe 😉

MichaelPascoe

Nice! Which techniques did you use? @MDesign

MDesign

https://forum.onshape.com/discussion/comment/112749#Comment_112749

my original suggestion. a series of unconnected sweeps that booleaned together after some tweaking of the ends and such with extrusions and a loft for the sharp corner at the bottom left.

eric_pesty

The "pattern and sweep" FS should let you do a bunch of sweeps from the same profile in one go as separate parts then you can boolean together.
This might a quicker way to get the end result.

dmytro_semenov

I'm certainly amtor. But could you show in more detail how you did the sweep. Even when I create a new one it still gives an error.

MDesign

That particular corner I needed to stop the sweep short (to avoid self intersecting) and apply a loft add with a curve guide to complete that turn. Also I used a triangle as the sweep profile and added fillets at the end and only a couple fillets in the middle when necessary. like prior to this loft feature.

Good to see you attempting to replicate.

dmytro_semenov

I think I'm making fundamental mistakes. Because when the profile is too large, it throws an error when sweeping. The action with the loft that you showed only worked for me with a new project. Thanks for your time)

MDesign

it’s not a fundamental mistake. Just a limitation of sweep that it can’t self intersect. if the radius becomes too small that any edge of the sweep has to travel backwards along the path to maintain its profile orientation… it will self intersect.

martin_kopplow

Self intersecting sweep is technically possible since at least year 2000, though possibly not in all modeling kernels. It is often explanined that the software then does not 'know' what is inside and what is outside. Well, that is a nice approach to help imagination, though self intersecting means it is inside twice, and that's still inside. Always.

dmytro_semenov

In your sketch, I noticed that it is better to intersect the sketch lines at right angles. This helped a lot. Thank you.

But you still need to work with the profile.