Convert Sheet Metal Body to Normal Solid Body?

[Anonymous]

I'm trying to export a sheet metal body as .step, however you cannot convert SM directly to component. Is there a way to convert a sheet metal body into a normal solid body to then turn into a component. My SM body in just under "bodies" in the browser, not inside of a component.

[paul.clauss]

Hi @Anonymous 

Thanks for posting! There is not a tool for this - usually, I see requests to convert the opposite way (imported solid to sheet metal).

I did find a nice trick for this - if you select the single sheet metal body and single resulting cell in a boundary fill operation creating a new component, it will create a solid copy.

With that said, component type designations will not be maintained through a STEP export and the export process should pick up bodies at the top level of the design. Have you tested doing a STEP export and then reopening the STEP file in Fusion? It should include all bodies and remove any component type (sheet metal, PCB) designations.

This will give you the entirety of the design in STEP format - you could then go through and delete any bodies/components you do not want to include in the new file when it is reopened in Fusion. Then export again for a clean copy.

[sergiu.andreeff]

Paul Clauss, with the ”Boundary Fill” solution you saved my life! Thank you!

[heeyrich]

Thanks again for this workaround, worked like a charm. Needed this to export a sheet metal part to a SolidWorks user, who could not correctly import any of the versions I exported for them using the normal means. Converting the part to a solidbody using boundary fill and exporting that way did the trick.

[Anonymous]

That is a nice trick.  I've ended up with sub assemblies containing multiple sheet metal components, but when doing cross sections or showing assemblies by component colour, it ends up looking a right mess of colours!  So being able to make a multi-body, but single component assembly from all these parts for presentations etc it's great! 

[t.navalinskas]

Sheet Metal mode requires Design History to be turned on. Turning the Design History off will automatically convert all Sheet Metal bodies into Solid bodies. For converting a single Sheet Metal part, one might save the design as new, remove other parts, and turn off the Design History.

[vanessadebono95]

thanks! solved my issue - I was able to cut away sections that were previously sheet metal. Appreciate it