Understanding: Extrude and Sheet Metal Face

[foolishgrunt]

I have a question that I'm sure would need a fairly technical answer, but I'm willing to settle for anything that anybody could possibly help me understand.

I have the above sketch. These are projected outlines of two bodies (all bodies are hidden for clarity), and the larger body is elliptical. I want to create a sheet metal face inside the closed loop formed by the intersection of the outlines, on the right side of the sketch. When I try to create a sheet metal 'Face', the outline is not recognized as a valid profile. But when I use 'Extrude,' the profile is recognized and the body is created.

Now if I go back and create new curves within the sketch to duplicate the outline of the smaller part, and terminate the ends with coincident constraints on the ellipse, 'Face' now recognizes the outline as a valid profile and creates the body. 'Extrude' also works as expected. So it appears that, for some reason, 'Face' needs to see those coincident constraints while 'Extrude' does not.

Here things get a little weirder, because what I really want is to offset the new profile of the new body from the elliptical outline by one material thickness, as seen above. If I manually draw a new ellipse that is one material thickness larger in both axes, 'Face' and 'Extrude' both recognize the profile as valid. But if I don't manually draw the new ellipse and I instead use the 'Offset' command to create the larger ellipse, 'Face' once again fails to recognize the profile while 'Extrude' command succeeds.

To my layman's understanding, there should not be any difference between the 'Face' and 'Extrude' commands when it comes to recognizing profiles. Is anybody able to enlighten me as to why they're behaving differently in my case here? I wish to understand so I can better tailor my workflow in the future to avoid hitting such roadblocks.

[mcgyvr]

Good question.. As they have been modifying the profile detection in the past few releases I'm going to guess that they have implemented it for the extrude function but have not yet gotten around to doing the same for the face command.. 

[JDMather]

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@foolishgrunt wrote:

1. If I instead use the 'Offset' command to create the larger ellipse, 'Face' once again fails to recognize the profile 'Extrude' command does.

2. To my layman's understanding, there should not be any difference between the 'Face' and 'Extrude' commands when it comes to recognizing profiles. 

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1. Offset of ellipse can create two different curves.

If you offset near the major or minor axis - a true mathematical ellipse is created (not equidistant curve).

If you offset away from major or minor axis - an equidistant spline curve is created (not a true mathematical ellipse.

2:42 in the video below...

2. I agree.  My guess is that the Face command is still using the old profile recognition scheme.

[mcgyvr]

And the trick/workaround that worked with old profile recognition we are talking about is to place points at each intersection.. Then Inventor will allow you to pick the profile you want.. 

[foolishgrunt]

Ah, I see what JDMather is referring to about the offset creating a different curve - it is a little different. So I guess now I understand why that may have thrown the Face command.

I'll also keep in mind mcgyvr's workaround for placing points at the intersections. Thank you both for chiming in, I guess now I'll just have to see whether Face's profile recognition improves in future releases.

[johnsonshiue · Accepted solution]

Hi! The behavior is indeed related to profile recognition. Sheet Metal Face is not yet leveraging the geometry-based profile recognition. It is still using the traditional constraint-based profile recognition.

For this case, you will need to add sketch points at the intersection (where the two curves intersect). Then Inventor Sheet Metal Face will be able to find the regions.

Many thanks!

[foolishgrunt]

So it turns out that part of my question remains. I was able to proceed with my work for the time being by creating a new ellipse in the face profile, but as JDMather pointed out, it's actually a different curve than the offset that I really want. So in the interest of accuracy, I went back and redrew the profile using 'Offset' this time. As you can see the profile is recognized by the 'Face' command:

However, the face fails to actually be created and produces the following error:

So for whatever reason, the face creation succeeds when using a larger ellipse to simulate the offset, but using the actual offset feature generates this error. Any ideas why? (And yes, 'Extrude' again succeeds where 'Face' fails.)

[johnsonshiue]

Hi! It looks like a bug. Please share the file here. I would like to understand it better.

Many thanks!

[foolishgrunt]

I reproduced the error by starting from a blank file, please see attached.

[johnsonshiue]

Hi! Many thanks for sharing the file! It does look like a bug. Face should work. I need to work with the project team to understand it better. In the meantime, you can use Extrude command and set distance to Thickness to create the face-like geometry.

Thanks again!

[mornay_venter]

Hi @johnsonshiue 

Why has this not been updated yet, that the "Extrude" and "Face" features work the same in terms of picking up geometry?

Regards 

[johnsonshiue]

Hi! The same profile recognition ability has been added to Sheet Metal Face command on Inventor 2024.

Many thanks!