Problem with Sheetmetal Unfold/Refold

[brendan.henderson]

Looking for reasons why and how to fix this. A full circle Lofted Flange makes a cone which is then ripped. This flat patterns okay. I then placed a large fillet on the corner of the rip to identify the Unfold Stationary Reference. I issue Unfold and select this reference, then add a sketch and Cut and run Refold. I select the same stationary reference and the Refold now creates a half circle cone and it's location is totally different to where the Lofted Flange features are. Totally baffling to me. Any ideas? Part attached in 2014 format and Screencast inserted for your viewing pleasure 🙂

[-niels-]

Seeing the same behavior in IV2015.
I even moved the EoP up above the fillet, started unfold and immediately refolded.
It gives me half the original part on the refold...

I don't know of a solution, i think you've discovered a shortcoming/bug with the refold function.

[brendan.henderson]

Thanks niels.

Further testing shows it has nothing to do with the corner fillet. I thought I had it figured when I increased the workplane offset for 2nd sketch in the Loft (which makes it closer to a cylinder) but even that started to break down at various angles.

[brendan.henderson]

Even more testing shows that it's not a Lofted Flange issue. I get the same result (offset geometry) on the Unfold using the below workflows :-

1. Lofted flange, rip, unfold
2. Revolved surface, thicken, rip, unfold
3. Revolved surface part derived into a Sheetmetal part, rip, unfold

Each of the above create geometry that is offset (on issue of unfold) from the original feature creation. Also I've noticed that that at a point yet to be determined as I decrease the cone angle (so closer to a cylinder) the unfold/refold performs perfectly. In contrast if I increase the cone angle (closer to a flat plate) that the unfold creates the offset geometry.

I've run out of ideas of how to create this part. Any ideas?

[brendan.henderson]

Found this on these forums from 2009. My cone when flat is more than 180 degrees so this "clipping occurs". Can't believe that 5 years (and releases) later this problem still exists. My VAR has confirmed that on 2015 this problem is still present.

Autodesk, please clean up your act. I don't need new features. I'd prefer fixes to existing bugs for the money I spend. I don't think this is too much to ask for?

Re: fold/unfold a cone shape

16-05-2009 07:35 AM in reply to: kdale2006

Hi Ken,

The issue you described has been logged as #1200183 in our database but I am not sure when a fix will become available.

This "clipping" effect after refold happens for cones with an angle > 180 degrees. So depending on your requirements, a possible workaround for refold of large angle cones could involve unfolding, modifying and refolding smaller angle cones separately. You could then join them afterwards (using mirror solid, perhaps).

[brendan.henderson]

Hi Ken,

The issue you described has been logged as #1200183 in our database but I am not sure when a fix will become available.

This "clipping" effect after refold happens for cones with an angle > 180 degrees. So depending on your requirements, a possible workaround for refold of large angle cones could involve unfolding, modifying and refolding smaller angle cones separately. You could then join them afterwards (using mirror solid, perhaps).

[brendan.henderson]

A workaround for this problem is to create a revolved surface and then thicken it. But the revolve must not be full type, try something like 359.9 degrees. This then unfolds and refolds perfectly.

[jmiastkowski]

Has a proper workaround every been found?  I am using Inventor 2018 and am running into the same problem.  

I have a sheet metal plate, that I fold (which changes the orientation horribly), then unfold, I then attempt to either sweep cut or chamfer the part and refold which fails every time.  The only solution I have found is to put the sweep cut or chamfer into the flat pattern and forget about accuracy in the larger assembly.

[johnsonshiue]

Hi! This issue is not yet fully resolved. In some cases it may work but in some other cases it does not. The issue here is that there isn't a static planar reference for Inventor to follow particularly with a cone. As a result, Inventor has to create a planar reference from the side faces, leading to flaky behaviors.

The reliable workaround is to have a small extrusion at the gap. The extrusion has to be tangent to the cone. When you unfold, pick the planar extrusion face. Unfold/Refold will work more predictably.

Many thanks!

[Anonymous]

Brendan,

   Inventor doesn't like edits to flat patterns. Try placing you cut on a mid-plane (via sketch) before making a flat pattern. You may need to create a sketch plane to get the orientation you need, might be a little tricky, but it should give the results you want. I just downloaded you part file and tried on the YZ plane and it worked fine with the proper cut options (I used extents all and the first direction option) and it showed up in the flat pattern. Of course I'm using 2017, but I'll post anyway. Hope this helps.