Unfolding an Elliptical sheet metal part

[autorestorer]

I am trying to flatten an elliptical sheet metal part, but have not been successful as of yet.

I have tried to Define A-side but Inventor 2015 crashes. When I try to Create A Flat Pattern I get Failure creating Flat Pattern or "Bend has only one side. Please check the Thickness settings in the sheet metal styles." I have checked my styles and they do match the thickness in my sketch. Would anyone have any ideas on what may be causing this error? 

[JDMather]

Your cuts are not perpendicular to the flat?

What process will you use to cut the flat?  Does it have an articulating head - or does is make only vertical cuts?

[autorestorer]

This is a doubler plate on the outside of a
Conical cylinder. There is a pipe that penetrates the cone and the doubler, this is why the cutout is not perpendicular to the doubler.

Can the part be done like this, or does the hole have to be perpendicular? I tried using the flatten part command, but it did not work.

[johnsonshiue]

Hi! It looks like the first extrusion causes the part to have inconsistent thickness. I use Thicken feature to create the main body to secure consistent thickness. After that, the part can be unfolded without a problem. Please take a look at attached part. Let me know if you have any question.

Thanks!

[autorestorer]

Can you explain how you added the thickness? Did you convert the part to a surface? I am new to inventor and trying to learn as I go, your help is greatly appreciated.

[johnsonshiue · Accepted solution]

Hi! What I did was simply create a zero-offset surface on one face. Then delete the extruded body (with bad thickness). Then create a thicken feature on the offset surface. It is just a quick way to show you that it can be done.

You could delete the extrude feature and recreate it as a surface. Then thicken the surface as a solid.

Thanks!

[autorestorer]

Thanks this worked, great. I tried this method on similar parts with the same results.