I'm trying to sweep an ellipse with a guide curve, but keep getting an error that says, "The intermediate profile # 2 could not be solved.", which tells me approximately nothing. Do any of you guys know what SW is complaining about?
Re: Help with guide curves
Posted: Thu Mar 21, 2024 4:07 pm
by len_1962
put the file up, what version of SW are you using?
Re: Help with guide curves
Posted: Thu Mar 21, 2024 4:10 pm
by Uncle_Hairball
Yeah, I should have thought of that. I'm using SW2023, SP5.
Re: Help with guide curves
Posted: Thu Mar 21, 2024 4:42 pm
by matt
You're also using a path, right? Is the center of the ellipse "pierced" by the path? I don't actually have SW installed right in front of me, so I can't look at your file. The GC also needs to pierce the ellipse point. Make sure you're using the correct option "follow path and first guide curve" unless of course you have multiple guide curves. The path controls the angle of the sketch plane. You can use the arrows in the interface to show the intermediate sections. The sweep w/GC works by creating a bunch of intermediate sections and then lofts them together.
Re: Help with guide curves
Posted: Thu Mar 21, 2024 4:57 pm
by Glenn Schroeder
I was able to open your file just fine, and it didn't show any errors, but I suspect it also isn't what you want. Sweeps can only follow a single path. I believe you need a Loft instead. I don't work with them much, but someone will probably be able to help.
Re: Help with guide curves
Posted: Thu Mar 21, 2024 5:46 pm
by Uncle_Hairball
matt wrote: ↑Thu Mar 21, 2024 4:42 pm
You're also using a path, right? Is the center of the ellipse "pierced" by the path? I don't actually have SW installed right in front of me, so I can't look at your file. The GC also needs to pierce the ellipse point. Make sure you're using the correct option "follow path and first guide curve" unless of course you have multiple guide curves. The path controls the angle of the sketch plane. You can use the arrows in the interface to show the intermediate sections. The sweep w/GC works by creating a bunch of intermediate sections and then lofts them together.
Yes, the center of the ellipse is constrained to the origin, as is the end of the path. The guide curve is coincident with the ellipse. Selecting follow path and first guide curve hasn't changed the results; The error remains.
It seems like such an easy task and yet...
Thanks for the suggestions, Matt.
Re: Help with guide curves
Posted: Thu Mar 21, 2024 5:47 pm
by Uncle_Hairball
Glenn Schroeder wrote: ↑Thu Mar 21, 2024 4:57 pm
I was able to open your file just fine, and it didn't show any errors, but I suspect it also isn't what you want. Sweeps can only follow a single path. I believe you need a Loft instead. I don't work with them much, but someone will probably be able to help.
image.png
Yes, I was trying to use the curve to the left of the path as a guide curve, but it won't work.
Re: Help with guide curves
Posted: Fri Mar 22, 2024 9:18 am
by TTevolve
The shape can not change on a sweep, it can rotate around the center and/or contort when using "keep normal constant" setting, but the shape never changes. To get it to jut out on the left side like your skecth shows you would most likely have to do a loft or a series of extrudes/cuts.
Re: Help with guide curves
Posted: Fri Mar 22, 2024 9:55 am
by Glenn Schroeder
TTevolve wrote: ↑Fri Mar 22, 2024 9:18 am
The shape can not change on a sweep, it can rotate around the center and/or contort when using "keep normal constant" setting, but the shape never changes. To get it to jut out on the left side like your skecth shows you would most likely have to do a loft or a series of extrudes/cuts.
Thank you for explaining that better than I did. This is why it needs to be a Loft (or series of Lofts) instead of a Sweep.
Re: Help with guide curves
Posted: Fri Mar 22, 2024 12:17 pm
by Uncle_Hairball
TTevolve wrote: ↑Fri Mar 22, 2024 9:18 am
The shape can not change on a sweep, it can rotate around the center and/or contort when using "keep normal constant" setting, but the shape never changes. To get it to jut out on the left side like your skecth shows you would most likely have to do a loft or a series of extrudes/cuts.
I think you are mistaken.
Re: Help with guide curves
Posted: Fri Mar 22, 2024 12:18 pm
by JSculley
TTevolve wrote: ↑Fri Mar 22, 2024 9:18 am
The shape can not change on a sweep, it can rotate around the center and/or contort when using "keep normal constant" setting, but the shape never changes. To get it to jut out on the left side like your skecth shows you would most likely have to do a loft or a series of extrudes/cuts.
That's not true. A guide curve change change the shape of the profile that was used to generate the sweep:
Re: Help with guide curves
Posted: Fri Mar 22, 2024 12:24 pm
by JSculley
The issue with this part is that SW doesn't like something about the relations in your profile sketch. If you delete them, the sweep with guide curves completes without errors. The trick will be to determine which relation(s) it doesn't like.
Update: After some further tests I see what's happening. You cannot have a relation that prevents the profile from 'stretching' to meet the guide curve.
Re: Help with guide curves
Posted: Fri Mar 22, 2024 1:36 pm
by TTevolve
JSculley wrote: ↑Fri Mar 22, 2024 12:18 pm
That's not true. A guide curve change change the shape of the profile that was used to generate the sweep:
image.png
Sorry, I stand corrected. I have never done anything like that with a sweep. I might have to play around with that some.
Most of what I have done in the past has been rectangle to round transitions which I don't think would work with the sweep.
Re: Help with guide curves
Posted: Fri Mar 22, 2024 7:35 pm
by Krzysztof Szpakowski
I think the problem is that the two profiles are slightly different (circle and ellipse) and there are inaccuracies in the drawings. In my case, I used the same Sketch2 profile and unchecked surface blending and it worked. I recommend being more precise and avoiding surface penetration like yours
Re: Help with guide curves
Posted: Mon Mar 25, 2024 12:29 pm
by Uncle_Hairball
Krzysztof Szpakowski wrote: ↑Fri Mar 22, 2024 7:35 pm
I think the problem is that the two profiles are slightly different (circle and ellipse) and there are inaccuracies in the drawings. In my case, I used the same Sketch2 profile and unchecked surface blending and it worked. I recommend being more precise and avoiding surface penetration like yours
image.png
image.png
I finally got it to generate the sweep. There was a small overlap of two splines that seems to have been the source of the problem. I never did, however, find a checkbox for surface blending. Where did you find it?
Many thanks for the suggestions!
Re: Help with guide curves
Posted: Mon Mar 25, 2024 12:32 pm
by Uncle_Hairball
JSculley wrote: ↑Fri Mar 22, 2024 12:24 pm
The issue with this part is that SW doesn't like something about the relations in your profile sketch. If you delete them, the sweep with guide curves completes without errors. The trick will be to determine which relation(s) it doesn't like.
Update: After some further tests I see what's happening. You cannot have a relation that prevents the profile from 'stretching' to meet the guide curve.
image.png
Thanks for the advice. I was able to get it to solve by removing an overlap between two curves.