I don't think that is a silly question at all Chris. Sure seems like there should be a way to save out the body and retain the sheet metal info. Of course you can still put your sheet metal bodies in a drawing and also dxf (or whatever method you use) out to flat patterns from the multibody environment but I'm sure there are occasions when you just want separate parts that have the sheet metal functionality and don't want to convert (again). I had never thought of this as much of an issue until recently. I have an 81 body part and 13 of those are sheet metal. My multi body part is full scale but I want to end up with parts that are 1/60th scale. In my case it is almost desirable to loose the sheet metal info since the scale has to be done prior to any sheet metal features. In case you wonder, my multibody sheet metal parts are 60x thickness and radius. In any case it got me, just like you, wondering why.
I have done multi-body sheet metal parts as one part file. I then use a separate (derived) configuration for each body. Then suppress the other bodies.
So Config A has bodies B & C suppressed; Config B has bodies A & C suppressed, etc.
I am curious as to why you "Save them out".? (I think I may be misunderstanding something about this process).
Your flat-patterns already exist as sheetmetal components in the Multi-Body part.
All the required info is in the Cut-List properties anyway. And, material thickness is easily added to the cut-list for detailed drawings and remains there and will update perfectly no matter what changes are made along the way.
Even large-ish Multi-body parts (of 200+bodies) don't take so long to process to dxf etc, and, it all remains parametrically linked in one neat part file.
Plus all the individual sheetmetal and Plate drawings also remain connected to the part, regardless of revisions.
The entire part is easily enough processed in a single multi-sheet drawing file.
And, this is the biggest win for me, It's all done with NO MATES to break or flip.!
So, yeah, why do you have to save them out and convert..?
very interesting. I will give that a try.
So how do you reference each "part" in a drawing? do you make a config of each body in the multi-body part file? I could have 50 to 75 bodies...thats a lot of configurations.
thanks for the input!
I do not use configurations for this. That's way too much fuss. lol.
(And, the number of times I have changed a config, to learn I needed to practically create a new drawing to recapture it in the new config.)
Besides, folded and sheetmetal parts create their own "Flat pattern" configurations within the part file.
I will assume that they too are lost when "Saving the Part Out"
And because it is a part file after all, I simply use the select bodies option on the drawing file to select the individual body required.
Any plate or sheetmetal part that is not parallel to a default plane I will simply select the required dxf face and use "Normal to"
This permits the option of select "Current" view in the drawing view palette.
This drawing file will remain linked to that body regardless of any changes to the body. (Unless of course it is deleted and recreated differently.)
You can then drag a cut-list onto the sheet showing pre-assigned part no, quantity, thickness, material type, bounding boxes, etc.
Simply remove all other items from the cut list. This data will of course auto-update if one alters any relevant parameters. thickness, size, quantity, etc. Add a Flat-Pattern and Fold-Table and we're all good.
I then use these drw drawing files to make pdf's for the Laser-Cutting Service and track and locate the plate files when making changes.
I don't have all the answers. (I may even be making a lot more work for myself.)
But the manual data entry is fairly minimal. And, it works for me.
Now, I am trying to understand why you would "save the parts out"?
ie. How does that work.?