Sweep intersect itself error

[Anonymous]

Hi, 

I am creating a really simple phone case. I want to sweep my shape around the "phone shape". The problem I'm getting is that the shape will intersect itself on the corners, which I understand, but is there a way of sweeping anyway? Is there an option to just 'blend' the intersect into the design per se. I have added some screenshot below, as well as a screenshot of what I want to achieve. Any help is appreciated. 

Thanks

Iwan

[TheCADWhisperer]

File>Export and then Attach the *.f3d file here.

I would probably create as a solid and then Shell or as a surface and then Thicken.

[jeff_strater]

a solid sweep cannot self-intersect, and there is no way around that in Sweep.  Listen to @TheCADWhisperer for better approaches.

[Anonymous]

Thank you! Curious to see what you come up with. 

[TheCADWhisperer]

You have some pretty "rough" splines in your sketches.

[Anonymous]

Yes, correct. 

[Anonymous]

Did you manage to overcome this problem? I cannot open your file because (I think) I have a student version, and Fusion is asking me to update, but there are not updates available it seems. 

thanks

[Anonymous]

Hi again, 

Okay, so from your comment, I re-drew the rectangle, then used the circle tool to create the corners. This worked, thanks. 

The reason I didn't do this first time, is that I wasn't sure if the corners had a constant radius'. I hope that makes sense. See image attached. 

To add, do you know why a 'rough' spline wouldn't work? I've seen tutorials online of a Loft working fine on a Spline similar to mine.

Thanks again for the help

[TheCADWhisperer]

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@Anonymous wrote:

I've seen tutorials online of a Loft working fine on a Spline similar to mine.

Make the splines tangent continuous and they will work fine.

Use as few points in the spline as possible (yours need only beginning point and ending point and tangent).

[TheCADWhisperer]

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@Anonymous wrote:

 I have a student version, ... but there are not updates available it seems. 

Any issues have nothing to do with your license being a student license. Are you running on Mac or are you running on Windows machine.  

If Windows, search your machine for file named Fusion 360 Client Downloader*.exe

[TheCADWhisperer]

This spline is particularly poor quality...

[Anonymous]

Thanks

[GRSnyder]

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@jeff_strater wrote: a solid sweep cannot self-intersect, and there is no way around that in Sweep.

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@jeff_strater, is this not a self-intersecting Sweep?

Here it is as a pattern of extrusions along the same path, which shows the intersection more clearly:

I'm sure the limitation has something to do with intersecting geometry, but it must be something more specific than just "two 'stations' of the swept profile cannot claim the same point in 3D space". No?

Edit: In fact, even this self-interpenetrating result seems to be allowed :

[jeff_strater]

@GRSnyder - you are definitely right.  Apparently, my information was sorely outdated.  What seems to be the case is purely analytic geometry (lines and arcs) seems to allow self-intersections, but a more complex path, like a spline, does still have this restriction.  I do remember, now that you mention it, hearing about a kernel improvement a while back that would allow self-intersections in some cases.  I apologize for the misinformation...

[GRSnyder]

Thanks, @jeff_strater, good to know!

The case that set me on the path of investigating this does indeed involve splines, both for the profile and the rail. So it's entirely plausible that this might still be the important distinction. It's a confusing problem to run into because the error message explicitly talks about the issue being self-intersection, and yet the canonical example of a Sweep is often something like the 90 degree pipe bend shown above.

[r.mitschke]

Maybe you can try to use the sweep command in the surface tab instead of creating a solid. I believe that surfaces can self-intersect, while solids cannot. 

[Imonacomputer2004]

(Sorry to necro)

This just saved some of my already thinning hair. Wanted to ignore a sweep in which the path was too curvy for Fusion's liking. Made the sweep with a surface rather than a solid, split the body with the resulting surface, and removed the unwanted portion. Thanks!