Error when trying to convert to sheet metal to unfold cone

[lcolbur1B4RTS]

Hi all,

I am trying to flatten/unfold the attached cone, and followed what seems to be the correct process of adding a planar face, but when I try to convert to sheet metal, Fusion keeps giving me an error that it can't calculate body thickness. Can anyone please help me resolve this issue? Thank you very much!

[HughesTooling]

If you right click this face there's no option to create a sketch which means it's not flat.

I deleted this feature then created an extrude using the opposite face.

And now it converts. See attached file. It will unfold but the flat pattern gives an error, probably because the cutouts are not perpendicular to the face.

[lcolbur1B4RTS]

Awesome, thank you very much! I'll keep in mind that I can check to see if a surface is flat by whether I can create a sketch from it. It looks like the unfolded cone is correct to me - I didn't get an error.

[HughesTooling]

---

@lcolbur1B4RTS wrote:

It looks like the unfolded cone is correct to me - I didn't get an error.

---

Unfold works but flat pattern gives an error. A flat pattern will give you bend lines .etc and should export to a DXF but it fails with this part.

[lcolbur1B4RTS]

Copy and thank you. I tried again but this time I split the cone in a different spot. I was able to extrude a flat surface, but still can't convert to sheetmetal. Is my current configuration capable of doing so?

[Warmingup1953]

***EDIT__Correction***

Let me check again...Standby 

I fear that body is not conical. Can you share the full file with the sketches(?) that created the "Cone"?

The fresh blue two-point sketch line shows the cut cone is not conical.

[Warmingup1953]

I believe there was a geometry issue. I created a fresh thinner true cone then Intersect Combine with the original to transfer the penetrations.

Can you share your full file? My example will need testing to ensure correctness to your intent.

[lcolbur1B4RTS]

Interesting. I tried to recreate the cone but still no luck. I've attached my full file. Thanks for your help.

[Warmingup1953]

This is quite messy, any reason it is not a single line?

[lcolbur1B4RTS]

No reason other then I'm more of a novice user. I've attached a cleaner version. Still no luck converting to sheet metal.

[jhackney1972 · Accepted solution]

For a Conical sheet metal body, to make the cut in the solid body, you need to use an angle cut.  If you look at my model, you will see a 1 degree wedge cut has been used instead of your straight cut.  The attached model can be used for a Flat Pattern and an Unfold.  You can move the timeline to get the unfold but you can also create another one if desire.  The small extruded edge is required and must be selected to do the Unfold.  Take a look at the animated GIF.

If this answers your question, please select the "Accept Solution" on my post. If you need further help, please ask.