Sweep Tool -- "Error: The sweep would create an illegal surface. ..." WHY?

[gruvin]

Howdy folks.

Seems the two parallel paths I'm trying to use just won't play together as path and rail. I mean, it doesn't seem to matter what profile I draw. I always get this error when trying to create the sweep. The paths themselves are to 3D projected edges, from a previously create, "coil" having square section.

But why?

😕

Any ideas? Thanks!

[Beyondforce]

Hi @gruvin,

In order for the Sweep to work, the Profile and the Path must be connected to each other!

Cheers / Ben
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[PhilProcarioJr]

@Beyondforce

"In order for the Sweep to work, the Profile and the Path must be connected to each other!"

This is not correct, they don't have to be connected with a sweep. The guide rail is the one that has to be connected to the profile.

[PhilProcarioJr]

@gruvin

Your profile is probably crossing over itself, can you post your .f3d file so we can look at it?

[Beyondforce]

@PhilProcarioJr, you are right my mistake.
@gruvin, try to switch between the Path and the Guide Rail.

Ben.

[gruvin]

Thank you for the replies everyone.

Here is a shared link to the the design file with the problem.

First, I did a test of this theory, in another design file. It worked just fine ...

I suppose that both path and rail are, "connected" via the projection of each path to my sketch. But this is also the case in the latter, problematic version. It still does not work.

Then I repeated something similar, but more accurate profile in the main design.

Here we can clearly see that both paths are, "connected" -- or rather projected into the profile sketch.

Concerning the possibility of the profile crossing over itself, I tried a simple shape ...

No joy there, either.

Before this version, I used paths horizontally adjacent, instead of the presently vertically aligned couple. It makes no difference. The two paths come from the edges of a previously created coil ...

I also tried a triangular section, so as to get a guide rail in the vertical center of the profile sketch. Again, no difference. Same error.

Oh and I have tried switching path and rail selections, as well. No difference.

I can see no substantial difference between my test, which worked and this later version.

Oh! I think I do see a small difference. Actually, it is NOT the paths that are projected onto the profile sketch, but rather the square section upon which the sketch is drawn. Let me change that now, by projecting the actual path end point ...

 Alas, no change. Same error.

So now we have a single profile sketch, containing the profile and the two paths. Last clutch at a straw, then ... I'll try selecting the path from the original path sketch and the guide rail from the profile sketch, so as to keep them completely separate, in theory ... nope. Same (non)result.

Perplexing it is being. Jedi Master even so! 😛

[Beyondforce · Accepted solution]

Hi @gruvin,

Here you go.

I want you to notice 2 things:

1. The change that I have mad to the Coil section size.

2. Which line I have chose for the Path and which line I have chose for the Guide Rail.

Cheers / Ben
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[gruvin]

@Anonymous -- Thanks! Seems if I had just continued experimenting, I might have stumbled on the solution -- or not.

I still cannot fathom any reason why reducing the section size of the base coil should make any difference -- and I cannot see why the selection of path versus rail should make any difference, in this case. But I suppose we'll just have to accept those oddities and move on.

Thanks again.

[Beyondforce]

I'm not sure, but it could be because of the limit of, how close the profile can be crose itself. You have a very pointy tips and with this round path they are almost touching each other.
So initially Fusion will check the spacing, and if it's too close, then it won't allow you to continue. But later on, it won't mind to get closer again.

That it's just my theory!

Ben.

[gruvin]

@Beyondforce ... yup, I think you're right.

I later changed to the negative of that pointy shape, such that there were now flat sides instead of points. The same issue occurs but is much easier (for me and for Fusion, I think) to cope with, by slightly lowering the height of the profile, such that it doesn't touch itself.

By using a negative cut sweep, instead of a positive join sweep, the otherwise broken surface issue, produced by the small gap was eliminated ...

All this to allow a GHT (garden hose thread) to be accurately modelled, since it's not available in Fusion's built-in list. This way of doing things almost directly models an actual thread milling operation. So, I suppose it's no wonder that it ended up working best. 😉

I originally tried the simple built-in triangular coil section, with fillets applied to the sharp edges, afterwards. I wasn't happy with that.

Adding a chamfer to the resulting thread entry was done using a cut loft between two discs ...

... this being the final result ...

Well, hopefully that helps someone, some time. I changed this thread's (no pun intended!) title to aid in potential, future searches for, "thread" etc.

Thanks again -- to all who contributed here. Really appreciate it.

Bryan.

[Beyondforce]

Hi @gruvin,

I would like to know what @jeff_strater thinks about my theory? 

"I'm not sure, but it could be because of the limit of, how close the profile can be crose itself. You have a very pointy tips and with this round path they are almost touching each other.
So initially Fusion will check the spacing, and if it's too close, then it won't allow you to continue. But later on, it won't mind to get closer again."

Ben.

[Beyondforce]

Btw, Since you like to work with threads. I have made a few videos about threads and this is one of them, I hope you like it:
https://www.youtube.com/watch?v=ngJPpCpg6zs

Ben.

[jeff_strater]

Hi @gruvin and @Beyondforce,

Sorry for not getting to this sooner.  My guess is that it could be a couple of factors.  First, what @Beyondforce says is a good candidate.  If the profiles are very close to touching, then the sweep could self-intersect.   I'm not exactly sure why it works sometimes and not in others.  It could be numerical variance.  

I've also been working with Matt on this thread:  sweep-tool-nightmare, and that design also uses a path + a rail.  We have identified what we think is a bug in Fusion.  You can see in the examples there that, even with the rail, the sweep goes wonky at some point.  I wonder if this is the same issue.  I downloaded the "bad" design, but it seems OK to me, so you much have gotten it to work eventually.  I'd be interested in the bad design, to see if it is the same as Matt's problem.

Jeff

[Beyondforce]

Hi @jeff_strater,

Thanks for pitching in. I also want to add, that the error we get, doesn't really say anything about profile intersection or any other reason for that matter.

 I wish the error was more detailed, with enough information to help troubleshooting.

I have attached the problematic file.

Ben. 

[jeff_strater]

It does seem, at least on the surface, to be related to the other sweep problem.  I notice that the sweep will succeed at .1226 (distance along the path) on this model, but fails at .1227.  This is right where the sweep makes its first full circuit:

If you zoom in, it certainly looks like there should be enough room for the sweep not to self-intersect:

And measure proves this:

So, as far as I can tell, this sweep should succeed.  When we get the change that we think will fix the sweep in the other thread, I'll try it on this one, as well.  Thank you for sharing the design.

Jeff

[Beyondforce]

Thanks for looking into it. I know it's a tricky one 🙂