Sweep failing to calculate when cutting and the path loops tightly.

[rfisherRR56Y]

I am having a tremendous issue with sweep not following a 3d sketch. It seems that fusion is throwing a fit whenever the profile would touch itself it were all layed out at once. I would understand this from the point of creating a solid body (although I would still think it would just know for sure that part is solid), but when it is cutting and this error is thrown it's utterly ridiculous the software loses it's mind because an area is cut twice. Assuming that is the issue of course. 

All that being said, Autodesk do you have any answers to this problem that wouldn't be a question in SolidWorks? 

[g-andresen]

Hi,

Without insight into the design (f3d) there will be no useful clues.

Please share the file.

File > export > save as f3d on local drive  > attach it to the post

günther

[rfisherRR56Y]

Hey Gunther, thanks for getting back. I actually can't upload any images as it is protected IP. Sorry for the bad news.

[TheCADWhisperer]

@rfisherRR56Y 

Can you make up a dummy file that exhibits the same behavior as your proprietary data?

[rfisherRR56Y]

This should work. I had to sweep in two goes. The first sweep worked but the second would not and I am not sure why. 

[jeff_strater]

yes, Fusion does not allow self-intersecting geometry in a sweep. 

"I would understand this from the point of creating a solid body (although I would still think it would just know for sure that part is solid), but when it is cutting and this error is thrown it's utterly ridiculous the software loses it's mind because an area is cut twice."

Cut is achieved by building a solid "tool body" and subtracting it from the target body, so the limitation is the same for body creation, addition, subtraction, intersection.

[rfisherRR56Y]

Hey Jeff, 

I appreciate the look under the hood and I suppose that makes sense as to how the cut operation is performed, although to my incredibly limited programming knowledge it seems computationally expensive. Either way, the more I think about it the less it makes sense to me that a solid body could not be created whenever a profile wraps on to itself. I would think the software would realize the body is already solid at that point, and instead of throwing an error it would simply know it is still solid. Same way when if you are joining with extrude you can you extrude into the body a fair way past the surface and it will just know that part is solid. 

I suppose that is all pie in the sky conversation in the end however. For now, I am constrained by an outside print to the path and size of the groove. So is there anyway to get this to work in the meantime? 

Thanks again, 

Ryan

[jeff_strater]

This is just a limitation of the modeling kernel - self-intersecting geometry is not allowed within a single body.

"Same way when if you are joining with extrude you can you extrude into the body a fair way past the surface and it will just know that part is solid. "

Yes, but that intersecting geometry is between bodies (the target body and the tool body), and the intersections are then trimmed out as part of the join/cut operation, so that there is no remaining intersecting geometry in the resulting body.

"So is there anyway to get this to work in the meantime?"

Sometimes, you can create multiple sweeps so that you can force it into then being more like the case you describe with Extrude.  The case in the video below is an example.  It doesn't always work, though, because you have to be able to isolate the area of intersection.  If this is caused by a single curve where the radius of curvature is less than the diameter of the profile, it will be harder, or maybe not possible.