Error: The operation failed due to a self-intersecting Surface

[Anonymous]

I created a t-spline body that refuses to convert.

It's a series of crossing curves, piped out in the Sculpt environment (as you can't pipe multiple curves in the Model env):

When I try to convert it, it errors out with "Error: Conversion error for: Body7
The operation failed due to a self-intersecting surface. Try adjusting the values or changing the input geometry."

Reviewing it in box mode doesn't help me figure out what's wrong, and how to resolve it. 

Any ideas how to get to the bottom of this? 

I'm attaching the design file.

[jeff_strater]

I am looking at your design.  I think I found the problem.  More updates soon.

Jeff

[jeff_strater]

Hi @Anonymous,

I found the self-intersection, and it is valid.  If you click on the error, it highlights the intersection.  However, in this case, the intersection is very small, and hard to see at first:

(the arrows are mine).

Zooming in, you can get a better view:

I cut down the model to make it easier to deal with, but here is how I repaired it:

In box mode:

I had to do a bit of moving of edges and faces in Edit Form to get this untangled.  I did this in box mode:

I'm not sure how you expect this to look, so I just got the errors to go away:

And, it converts OK

However, stepping back, I understand your statement about the Pipe command, but I would not recommend using Sculpt for this.  This model, even in its incomplete state, it is very slow to deal with. This is a fairly large Sculpt model, and it is clearly straining the compute.  Unless you need to edit these "pipes" using Sculpt capability, I would not do it this way.  I would do this as a solid model, and use sweep, or separate Pipe features, and Combine to join them together.  It's up to you, of course, but it's something to think about.

Jeff

[Anonymous]

Thanks Jeff,

but I'm afraid you used the wrong model.

I've updated the post immediately after posting it with a new file -  potter v10.f3d

The body name should be Body 7 and the error is different (Self-intersecting surface). Can you have a look at that one? It's probably the same problem area, but is it the same solution? 

Regarding not doing it in Sculpt - I wish I could, but there are 50 curves projected, and in solid mode I can't do it more than one curve at a time. (Is that a bug? or by design?)

And you can't join curves either on fusion... 

Compare this with Rhino, that does all of it at once and in a few minutes, and see why I was really trying to find a solution that works similarly on Fusion... 

[jeff_strater · Accepted solution]

The error is the same.  In addition, there are two more errors, which were probably there in the original model as well, but I never took it that far.

Here is a screencast of me fixing the model.  It should give you an idea of some ways to "untangle" intersections.  It's a bit long, but that's mostly because of the delay caused by working with such a large TSpline model.

Finally, I went through and created solid pipes from your sketch lines.  I agree that Pipe should allow selection of more than one curve at a time, which would make this a whole bunch easier.  I will add this suggestion to our backlog.  But, I think the performance of this model will be significantly better than the TSpline version.

However, even if we allow multiple selection, Pipe will still be fairly basic.  It's not the same as a frame generator.  That's a longer term requirement

Hope this helps

Jeff

[Anonymous]

Thanks Jeff! I'll watch it later today.
Thanks so much for your help, and for adding it to the backlog!

[Anonymous]

Jeff, how long did it take you to pipe each of them individually in the Model env? 

[jeff_strater]

I don't really remember how long it took to create the solid pipes.  It was pretty quick - 5 minutes, maybe?  The bigger problem is that you then have a lot of features in your timeline.  You can collapse them into a timeline group, which helps.  I also created them with a parameter for pipe diameter, so I can change the size all at once.

BTW, I found out why Pipe does not allow multiple curves to be selected.  It's because of the "hollow" option.  If I have a simple sketch like this:

And create two hollow pipes using these lines, you get unexpected results:

That is, the pipes are not hollow all the way through.  We could maybe fix that over time, but that's the reason why it was not done at first.

The other option is to allow multiple selection for solid pipes (your case), but not for hollow.  That UI might be surprising to people, though.

Jeff

[Anonymous]

Can we just gray the hollow option out, and/or explain in a tooltip?
Seems like it would be worth it.