Cannot unfold sheet metal

[KevinMacDonald]

I am experiencing erratic behavior with sheet metal. Here is my workflow:
 - From a sketch I extrude a surface using one or more tangential arcs. I am extruding perpendicular to the sketch. The surface only curves in one direction.
 - I then might using other surfaces to split faces of that extruded surface to arrive at a surface that I want to convert to sheet metal and unfold.

 - I thicken the surface.

 - I use Extrude to create a small flat tab to use as the stationary face for unfolding.

 - I convert to sheet metal. 

 - I then try to unfold. SOMETIMES this has worked fine. And now, it fails consistently. Fusion will not allow me to select the stationary face. It does not highlight. 

The above workflow has worked completely fine SOME of the time. And in my design I cannot do even the simplest unfold. I have tried using a new sketch with new geometry. I have tried making a component of my surface first, and then thickening and turning it into sheet metal. I see a Sheet metal rule show up in the component. Fusion seems to connect the thickness and match it to a rule. But I cannot get past the unfold step. 

What do I do? If I cannot get past this problem then I have a design in an inconsistent state and I cannot move forward with any confidence. I will pay for tech support if necessary.

Thanks

[davebYYPCU]

Works if the Press Pull is suppressed.

Will presume the resulting face is not radial to the curve.

Might help....

[KevinMacDonald]

Sorry, could you elaborate? Are you doing a press pull, followed by an extrude to create a stationary face? And then you suppress the press pull to unfold? 

The reason I am doing the press pull is simply to pull the body back from interfering with the other body it will eventually be welded to. At the end of the day I want the piece to be the right length, and to contain whatever holes etc. that I added to the unfolded piece. I'm trying to understand how suppressing the press pull gets me there. I may be unclear on what suppressing does or how it helps me. 

[davebYYPCU · Accepted solution]

Press Pull was suppressed. 

Not active in the timeline. 

Your extrude was then performed on the original body by Fusion without error. 

Unfold then operates as expected, because the Press Pull was suppressed.  Stationary face MUST be tangent to the curved body.

You effectively only offset the original body face to cut to length required.  This body face is no longer radially aligned to the centre point of the arc.  

If you draw a line to the curve from the centre point to Split the Body, then an extrude will be Tangent to the curve and the Unfold will be successful.

In the pic, the cutting line is not attached to the centre point.

Originally, I wrote what I thought was happening, now I can show you (what I said and) why your original workflow will not work.

Might help...

[KevinMacDonald · Accepted solution]

Unfold will work on a series of arcs of different radii and center points as long as they are tangent to each other. The major requirements are uniform thickness, tangency, and gaussian curvature is zero (curving in one direction only).

In my case I think you put your finger on my main problem. Press-pull has subtle effects, making the geometry more complex causing unfold to fail silently. My workaround is to perform an extrude to create the stationary face needed for unfolding, and then while unfolded I use a sketch to create profiles to trim the sheet metal to the precise length. However, a weird hack I must do is to leave a little sliver of the stationary face in place so that the item remains foldable. In future, I will add a short flat surface at each end tangent to the curves, making press-pull unnecessary. 

You led me towards a solution! Thank you.