Thanks for all the input guys,
I managed to find a suitable solution to the problem!
Originally, I used "Thicken/Offset" command to make a hollow solid of the model hoping that it would successfully convert into a sheet metal part after I adjusted the default thickness in "Sheet Metal Defaults". But the bend command refused to function with my geometry. I even tried using the "Split" command to divide the part into individual sheet first and load them into their own part files. Now, the bend command did work, but it created very poor trainsitions between faces around bends that changed widths. Namely, they would maintain the width of the first face and then suddenly jut out at a 90° angle to meet the next which creates an ugly flat pattern and a bad mating surface for welding.
In the end, I found the best method was to use the "Thicken/Offset" command to create surfaces at the exterior of my solid model, make them exportable by right-clicking and selecting "export object", then importing them to individual part files with the "Derive" function under the "Manage" tab. I could then create sketches on each face of the surface with an outline of that face (which Inventor is nice enough to do automatically). After converting the part to a sheet metal part, each outline sketch can be converted to a sheet metal face that automatically connects to adjacent faces using the rules and thickness settings in the "Sheet Metal Defaults". Thankfully, it does a MUCH better job creating bends with this method: each surface has a nice tangental curve connecting it.
This solved the issue of cutting the design into mutliple pieces and overcoming the bend command, but I still had to offset some of the edges on each piece to make room for the thickness of adjacent panels (since each piece was the exterior surface of a box extruded inward, adjacent faces generated by different surfaces would overlap). I tried sketching on the faces after converting to sheet metal, but the complex geometry around the bends prevented the "offset" sketch command from having a dimensionable offset distance. Additionally, since each edge was originally a sharp angle, and the new parts had curved bends, the mating edges wouldn't match if they were left in their current form.
Instead I went to each part that would overlap an edge, and created an exportable surface on the new interior faces again using the "Thicken/Offset" command. Then imported the surface into the part that would be overlapped. Then I could use the "Trim" function on the base surface using the imported surface as the cutting tool to perfectly match the edge to the its mating surface.
Ffter each surface was trimmed and converted to sheet metal, I could finally make the flat patterns I need.
Well that only took 6 hours.
Again, thanks for all the help!
