Can anyone explain to me why this part won't unfold?

[Anonymous]

Hi all. 

I've got a part (several actually) which I've imported in IGS format, because it was initially designed in another piece of software. 

9 out of 10 times I do this, I'm able to clean up the solid to the point where I can unfold with the sheet metal tools in Inventor.  Although I have quite a bit of these files to unfold, this workflow is fine for me.

Occasionally I have one (such as my example) which I just cannot figure out where the discrepancy is in this solid.

Does anyone have a surefire method of cleaning these types of files up that will eliminate this issue? 

I can just make it over from scratch with the sheet metal tools, but for future reference, it would be nice to know if I can avoid that. 

I appreciate any suggestions.

Thanks

[TheCADWhisperer · Accepted solution]

Does Manage>Rebuild All return any errors?

Are all cut edges perpendicular to the flat?

[kelly.young · Accepted solution]

Hello @Anonymous I see that you are visiting as a new member to the Inventor Forum.
Welcome to the Autodesk Community!

The method @TheCADWhisperer used by Delete Face > Thicken is by far the best way to accomplish imported solids to a Sheet Metal Flat Pattern. 

Another not as elegant way is to:

• Use Feature Recognition to get the outside shape as a Sculpt (without the Fillets)
• Project Geometry of the bottom face
• Create the side Flanges (use measure on Sculpted Solid for any distances)
• Extrude Cut To for the front angles
• Extrude Join To the angled plane for the back angles
• Extrude Cut To the little end notch
• Unfold
• Extrude Cut to remove the twisted sections
• Refold
• Create Flat Pattern

The flat patterns are fairly close, different ways to go about the same thing so thought I would show the scenic route. 

Please select the Accept as Solution button if a post solves your issue or answers your question.

[Anonymous]

Rebuild All did return an error: No edges found while making fillet feature. 

Cut edges are not all perpendicular, but that alone usually doesn't seem to hold me up.  The only problem being that I need to be careful which edges I'm projecting when making a flat pattern!

Thank you, TheCADWhisperer, for the input!

[Anonymous]

Delete Face > Thicken.   

That did it.  Oh, and it was right in front of me the whole time!

I now feel schooled.

That is one little time saver I will use quite frequently. 

Thank you @kelly.young and @TheCADWhisperer.