Sweep a solid around a complex surface

[skull]

I've made several attempt to sweep my profile around a complex surface to no avail. Guide surfaces etc, nothing helps. In the file attached you can see a small solid which represents an aluminum extrusion. I want the shape to go around the edge of the surface in the file. I've had a few semi working solutions. 

Can someone please assist. The ruled surface in the ipt I've been using as a guide surface and the larger surface is what I want to sweep it around.

Any help would be great! Thanks!

[johnsonshiue]

Hi! I am sorry I am a bit confused with the design intent here. You want to sweep the detailed solid body around the boundary patch surface. The solid body is well-defined. But, BP is kind of like a Freeform feature.

Without trying, I know the Solid Sweep will fail for sure. Are you trying to create the Rim? I think you need to use Profile Sweep instead.

Many thanks!

[skull]

The intent is to do a profile sweep. I do a 2D sketch on the small piece and project geometry to get the profile. This small piece is derived in so that this profile can me used in multiple parts but still controlled from one location. 

Can you try the sweep and see what I mean?

[JDMather]

This doesn't address you issue, but are you aware that you can Derive in an existing sketch as well (without deriving a body)?

I think the confusion is that you stated "Sweep solid" which is a new command in Inventor 2020.

I would have either - Derived the sketch only or hide the solid body after projecting the edges of that body, and left the word "solid" out of the discussion thread title.

Now that that has all been cleared up - maybe someone will devise a solution to your problem...

[j.palmeL29YX]

Are you looking for something like the attached? (Not yet complete. First I try to understand what you want to achieve).

[skull]

Yes. I'm able to get it to sweep along 3 sides like you have. But when you include the fourth side to close the loop it crashes.

[skull]

I wasn't aware of the sweep solid feature in 2020 as I'm using 2019 so it didn't even cross my mind as a point to clarify since in 2019 you're only able to sweep a profile. I was aware of the derive sketch. But for better or worse we've always just derived in the solid here and turned off visibility on it if weren't not able to Join during a sweep.

[j.palmeL29YX]

If you use a not closed 3D-path (build a small gap)  you can also include the 4th side in the path. Of course then you have to close this gap. (in the attached example i created a small loft). 

[skull]

Very cool. I'll try that! It's weird that it won't just do it.

[skull]

It didn't work when I tried it. Can you please share the file in which you were able to get it to work with the break?

[j.palmeL29YX]

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@skull wrote:

Can you please share the file 

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Sorry, I use Inventor 2020, you can't open my file. 

Maybe some Images will help:

- I splitted the surface anywhere to get a break in its boundary. 

- Sweep along the outer edges (not the broken curve)

- repair the gap (this can be a little tricky depending on the current situation. 

This is not an universal workflow. Sometimes you can get a acceptable result, sometimes it will fail or the result is not to use. - depending on the current geometry. 

[johnsonshiue]

Hi! Indeed, this is not a simple case. There are multiple issues here. The profile is too complicated. The sharp corners along the path can lead to unresolvable intersection.

I am able to simplify the profile and round the corner to get something close (see attached file).

Many thanks!

[j.palmeL29YX]

Here a new attempt with a result close to your goal. 

The >>first video<<  shows how to create the first two opposite profiles using the loft command.  (Before starting the video I created a sketch block including your given geometry). 

The <<next video>> shows how to add a mitre at one end of a profile. Repeat this at all four ends of the first two profiles. 

Now I created 4 simplified 2D-Sketches at the faces of the mitres (see attached image). I left out all the fillets from the sketch, because the following loft will fail if the sketches include the fillets). 

At last create two lofts along the long sides using the given rails and add the needed fillets. 

Done. 

(an .stp file is attached, so you can check the result). 

If my reply solves your problem, click the "accept as solution" button. This can help others find solutions faster

[j.palmeL29YX]

For those who are interested here the Inventor 2020 model.