The sweep would not create a valid result

[gom160-sld]

Hello,

I am trying to do something which I think is quite simple, and it fails, so I am thinking I am doing it wrong.

I am importing some svg shapes in a sketch, which I am using as a base for a design. In the example attached here, there is a beginning of a sweep. However, when I try to go further on the path it is on, I get this "The sweep would not create a valid result" error message (see screen capture, path outlined in blue).

The path is quite simple, there is no gap, nothing weird I can see. I'm new to Fusion, been playing with it for a few weeks, and have been running into that very issue a few times.

Can someone point to what is wrong?

Also, that sweep is supposed to branch out later on on the smaller inside path (also selected in blue in the screen capture). But Fusion doesn't seem to see that the outside and inside paths are connected. Any pointers?

Thanks for your help!

[Warmingup1953]

It appears your paths are not smooth...perhaps recreate them in Fusion 360 using lines and tangent arcs

[Bunga777 · Accepted solution]

I think it is because the curves in this section are not tangent.

You may want to rebuild the spline.

The last part was connected with Revolve.

We have tried to modify it to maintain the original shape as much as possible, please see the video.

https://knowledge.autodesk.com/community/screencast/ea7d4cd8-2454-4884-bfa4-1f9760258c93

[gom160-sld]

Thanks for both your answers, and thanks for going that far in the details!!! I was not expecting this level of help, thank you so much for taking the time!

I was thinking I needed to recreate the curves the way Fusion wants it, but I didn't know how to do it efficiently. Your video is worth a 1000's words.

Concerning the heart of the issue, it seems that some info is lost when importing the svg (attached here, I scale it by 4 when importing). I was careful in making the nodes smooth (except the pointy end, which has to be this way), I would think that this would result in tangent curves, but it is not the case... Is there a better way to import this file, or the method described here (import with issues, recreate curves under Fusion) is the best way to go?

Thanks again for your feedback!

[davebYYPCU]

How much time is being saved by importing an svg that does not suit Fusion in a fully compatible way.

Much quicker to sketch in Fusion, using constraints and dimensions as originally intended.

Svg bring more trouble than native sketching.  If you have too, import svg and extract projected points to a native fusion sketch and complete this new sketch by snapping to the projected points.

Might help.....

[gom160-sld]

Hello,

So I am trying to reproduce what was done in the video, and hit another problem.

I have recreated all curves in Fusion, making sure all curves are tangent. But I still cannot complete the sweep.

If I try to add the small curve highlighted in blue in this screen capture, I get an error: " The sweep could not create a valid body. Try changing the profile or path, or adjusting the operation values.".

Is there still something wrong in the sketch I recreated? Thanks!

[laughingcreek]

putting profile on the outside of the curve will allow sweep to bend around all the corners in one go-

[gom160-sld]

Thank you! Is there a way to replicate the curve I want to follow, but smaller, with a fixed offset towards the inside (so I end up with the same outline in the end)?

Thanks.

[laughingcreek]

there is an offset command in the sketch environment.  you have to be careful using it with splines b/c it will sometimes cause janky curvature that can cause subsequent commands like sweep and loft to fail. (there's a work flow to over come that issue).  generally, avoid offsetting splines, and always check curvature with a curvature comb.  offetting the path -1.3 and using that for a path worked in this case though.

[Bunga777]

Sorry for the late reply.(I have a feeling this has already been resolved. ......)

The reason why the sweep stops in the middle of the file you pasted seems to be a problem with the location of the sketch cross section.

Moving the position of the plane to near the middle will solve the problem.

[gom160-sld]

Thanks @Bunga777  for the info concerning the sketch plane placement. I am a bit perplexed as to why that is, I guess this is just one of this software's quirk? In any case, I will play with that next time I encounter this problem.

@laughingcreek, once you run a curvature comb on your sketch (documented here https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-DAAFFB13-712B-443D-B8E7-EE305BCE7F33 if anyone faces the same issue), what are you looking for, how would issues pop up?

[laughingcreek]

a basic spline curve, decent curvature (as observed by the curvature comb)-

offset that spline and we see there is a bit of jiggle in it-

you can't see that with your eye, but fusion can.  and will try to sweep/loft/etc along that miniscule jiggle, possibly causing an illegal surface, and thus a failure, in the process.

you can over come this by using surfaces instead.  extrude origia curve, and offset the surface instead of the sketch element.  here you can see the result of both laid on top of each other.  the offset surface is clearly smoother-

[gom160-sld]

Oh so it's sort of a derivative function of the curve's direction... Nice, thanks again for all the help and info!