Cannot create a flat pattern and can't find the problem.

[Anonymous]

I created this bracket, which is fairly simple aside from the odd shaped cut on the flange.  I tried creating a flat pattern but got an error, so I thought it was possible one of my cuts was to blame, so I tried it with both cuts suppressed at the same time as well as individually and it still gave me an error.  I don't get it.  Its 3 flanges; how much simpler does it get and why isn't it working?  Its making my brain hurt (yes, a Monty Python reference).  Please help!

[philip1009 · Accepted solution]

Flanges 2 and 3 are technically touching each other, separate them a bit and it will flatten out.  I agree it's annoying that Inventor can't tell that the flanges are supposed to be separate.

This isn't the problem with this part, but for general practice, use Cut under the Sheet Metal tab instead of Extrusion and Corner Round instead of Fillet, sheet metal parts can get glitched and weird using tools outside of the sheet metal environment if you're not careful.

[Anonymous · Accepted solution]

You are RIGHT.  THANK YOU!  I never would have even considered this, not in a million years of staring at it.  I separated the flanges by 0.0001 in and the problem is went away.

I have to say to the Inventor programmers (if you are listening), this kind of error is seriously aggravating  and you should fix it ASAP.  If it can create two flanges that touch (to be spot welded) it should be able to unfold them.  If it cannot unfold them, then when the flange is created it should introduce an infinitesimal gap so it can be unfolded, or it should give you a warning that the file may not unfold if the flanges perfectly touch.

The thing that really bugs me (no pun intended) is that this hasn't always been an issue.  I have created flanges that touch many time before, without a problem.  If I didn't have so many files in inventor, I would seriously give other programs a try.  I don't think they could be any worse and they certainly aren't more expensive.

[SBix26]

It has always been an issue.  I've been using Inventor since version 5.3, and I have never been able to create unfoldable sheet metal models with coincident faces.

Other programs undoubtedly do some things better than Inventor, but also vice versa.  Some of them absolutely could be worse for a particular workflow for a particular user, and some could be better.  It's highly subjective in many ways.  In this particular case, allowing for coincident faces in sheet metal is one workflow where Inventor falls short for many users.  It's a specialized workflow, though, and we definitely don't want non-sheetmetal parts to allow coincident faces within the same solid.

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Sam B
Inventor Pro 2019.2 | Windows 7 SP1
LinkedIn

[philip1009]

At least it's easy to fix flat patterns outside of Inventor, just put the thickness of material back into the flange in Autocad before giving it to the programmer.

[Anonymous]

I may be wrong, but I made this part in several variations over the years and don't recall having this problem with previous versions.  Its entirely possible i just forgot about the issue. 

[philip1009]

At least that eliminates the possibility of this being just a 2019 issue.  I guess I haven't encountered this issue because I typically only use notched flanges to be welded, or I always put a gap in for tolerance since bench presses are only as accurate as the human operator.

[Anonymous]

I don't build in a gap because I assume the operator will make adjustments
as needed to get everything to fold. It would be interesting to test which
way would produce better quality parts. I can see a rational for both.