What's the deal with sheet metal and components?

[TriplePRanch]

I'm working on a design that includes a lot of sheet metal parts. I've got a few hours into the design now, and just discovered that you can't create more than one flat pattern per component. You also can't drag sheet metal bodies into a new component. This seems like a huge limitation. Are you really supposed to create a separate component for every sheet metal body? What possible reason is there for this? And is there any way to fix my design now or is my only option to start completely over?

[Warmingup1953]

I'm sure others will remind you of Rule #1 at the head of this Forum....You won't need to start again on "THIS" design but in future be aware of the One Flat Pattern "Feature". For the design you're on at the moment you can extract Flat Patterns sequentially deleting the old one as you go. Deleting may seem drastic but in this instance can be subsequently re-patterned if needed.

[TriplePRanch]

I thought I understood rule #1, and do create new components for all of my sub-assemblies, but will still have multiple bodies per component. I never thought I was supposed to create a new component for every body.

[laughingcreek]

1-create new sheet metal component.

2-with new component active, use boundary fill to copy one of the Sheetmetal bodies to the component. 

3-convert new body created with the boundary fill to a sheet metal part using convert to sheet metal.

wash and repeat for remaining parts.

[laughingcreek]

you will generally end up with one body per component. 

[jhackney1972 · Accepted solution]

Here is a Blog Article and Video on how to create sheet metal components from sheet metal bodies.

[TriplePRanch]

Thanks everyone, and thank you John for the workaround. I love Fusion and it seems so intuitive when I'm working with solids, but I've just recently had to dive into sheet metal and joints and it makes me feel kind of stupid sometimes.

It seems like you should be able to copy and paste sheet metal bodies, and it would take the rule with it. It also seems like having more than one flat pattern per component should be possible.

Oh well, from here on out it'll be one body per component for me. Thanks again!

[kevinwatts]

Hi John Hackney. I always enjoy your tutorials. Solid information presented logically and at a pace that everyone can follow.

I tried your solution using Boundary Fill. It worked on a simple file that I setup to try.

However, I have "hit a dead wall" in another project that I have already done a lot of work with. I kept all sheet metal bodies in separate components, except for one. In that sheet metal component, I created a metal body and used several sketches to cut the material. One of the cuts was to create a part that I need from first body. Now I can not separate the second body using Boundary Fill. I have tried other workarounds like Export, Save As to create an external part to import back. It imports, however, as soon as I import to the current project and the timeline runs through it recalculate it spits out errors.

Any other suggestions?

[jhackney1972]

Can you attach you model so I can take a look see?  If you do not know how to attach your Fusion 360 model follow these easy steps. Open the model in Fusion 360, select the File menu, then Export and save as a F3D or F3Z file to your hard drive. Then use the Attachments section, of a forum post, to attach it.

[kevinwatts]

Hi John,

To protect the IP I can not share the model.

The solution that I found was to make new sheet metal components and rebuild both parts/bodies from the copies of the original sketches and same elevation planes. That allowed me to also make adjustments and improvements that were not possible going back in the design without causing errors. Errors were caused previously as the bodies were created and then referenced by projection in to other drawing for other components.

Then hide visibility of the original component that contained both bodies.