I am using SW2014 SP5.
One method is to RMC on the Cut List folder in the feature tree and select Save Bodies.
This will save out each body as a separate file.
However, the saved bodies will NOT be sheet metal. You will need to perform a convert to sheet metal on each one and collect all bends.
If you have hole wizard holes you will need to re-establish these if you want them to be recognized as such. I create a sketch and convert entities of all the hole edges and then fill. I then use the hole fill sketch to define the hole locations of a new hole wizard feature. This maintains the parametric location. Yes, a real pain of a work-around. Perhaps this is no longer necessary in newer versions of the software.
Once converted to sheet metal, you will have an individual sheet metal part that will flatten.
To help clarify, we save our bodies out as described more to jive with out workflow than anything else.
Here, each body would be a separate part number. And each part number gets a drawing. And burying different part numbers inside of a part is not handled by Workgroup PDM - at least as far as extracting BOM information.
J. Mather's approach is valid. But it doesn't fit our company workflow and file management.
Daen,,, Sounds like you would like to have an assembly, of what you are showing, with individual part files. If so, how about deleting the base feature of each part you want to exclude from your part file (you can keep any necessary sketch geom) and then saving that to a part number of your choosing. Open your multibody part file anew and do it again for another part until you have all the parts saved. Now you have functioning parts of each with all the info you put in. You then can begin a new assembly and simply insert the new parts. Don't drag them in. Just select the part you want then green check. The parts will come in fixed and in their correct positions. So you may want to unfix then mate.
In your assembly file.
Here is a screenshot of a file I tested this on. Not as complex as yours but think it should work. This started out as a single multibody part file.
Edit:.. I probably should add that if end up with a bunch of dangling sketch geometry (on edge stuff), and it is too much of a chore to fix that, use delete bodies and live with that in your new part files.
When I follow your OP, where do the files get saved?
Never mind I found them.
You should also be able to create a Flat Pattern for each body and then select each one individually for drawing creation without writing out the individual part files.
On occasion - I have had trouble with that though and often have other reasons to have each body in it's own file.
Here is how I handle a multi-body sheet metal part:
1. I see you have 20 bodies, so in the Default configuration, do 20 separate Delete Body commands.
2. Now create 20 additional configurations. (Part01 to Part20)
3. Use Configure Features so that each Partxx configuration has its associated Delete body command suppressed.
4. Go back and suppress all those delete body commands in Default configuration. (This sequence saves on mouse clicks!)
4. Now create a drawing for each Partxx configuration. I have Sheet 1 as the bent shape.
5. Add a second sheet and insert the body, but select Flat Pattern. This will force SolidWorks to add the Flat Pattern derived configuration to the part file.
6. Repeat 4 & 5 for the other 19 parts.
In effect you have created 1 assembly and 20 part files in a single multi-body part file. I assign configuration-specific part numbers ,etc.
Now any changes in Default will be reflected in the Partxx configurations / drawings / flat patterns.
I'd be using #TASK for this.
If you just want the DXF's use the "Export Flat Patterns" task to export your multi body flat patterns straight to DXF.
Or if you want SolidWorks drawings from them, use the "Sheet Metal Drawings" task. It will create a single drawing file with the flat patterns on it. You could then use the "Drawing Splitter" task to separate into individual drawings if needed.
Yes, this has been a behavior of SW for.... every maybe. The typical work around for this is to add a very small straight section to your large curve to act as the base flange. Small means like 0.03". Enough that the software can use it but insignificant to your part. Yes, it does change your part dimension. But you can usually size the flat flange to be smaller than your tolerance.
I don't do Sheet Metal everyday like I did a few years ago..
I did try multi part sheet metal and I guess I'm too ignorant or too old school, or to set in the Sketch Part ways, but really isn't it much simpler just making individual parts? For individual custom properties, ease of parametric changes...........
My process is definitely NOT for everyone and it does have it's pains. Here are a few screen shots to help clarify a little more...
Here is a frame weldment with sheet metal bodies. The frame will be built in-house. But the sheet metal blanks will be laser / water jetted by a vendor.
The sheet metal bodies are saved out to separate files.
Here is the saved sheet metal body. It was converted to sheet metal. Next holes were filled. This is done for two reasons: SW looses Hole Wizard info when the bodies are saved and if you want to benefit from the parametric hole call out tool in drawings this is a necessary step. And sometimes holes need to be added AFTER the structure is welded.
At the end of this feature tree, there is another SAVE BODIES. This creates the BLANK part that will be sourced from the outside vendor. Remember, these steps are much more about process than the best or slickest way to perform this in SW. Since different vendors are blanking and bending (whether internal or external vendors) the blank needs to be separated from the bent part as far as part number and tracking. If we were to send this to a sheet metal shop that creates their own blanks and performs there own bends, then the whole "separate blank" process would not be performed because that is "their" internal process instead of ours. In that case we just order the part number of the bent form.
The corresponding drawing with a note calling out the use of an existing blank...
And here is the blank... "lather, rinse, repeat" regarding the convert to sheet metal and in some cases filling holes.
Is all this a ROYAL Pain in the Dark Side! Absolutely. But it is process driven. Managing this type of thing through configurations, which most of you do, would be much less initial work. The down side is that method buries P/N 456 inside of part file 123. We are still using Workgroup PDM and it does not have the ability to pull configuration specific BOM data - such as the P/N 456 noted above - for reports or importing into our ERP. You also loose the nice functionality to open a drawing by Right Mouse Clicking an open part/assembly and selecting Open Drawing because the drawing for the sheet metal is a different file name than the drawing for the multi-body part. The use of a single drawing to contain all the drawings for all the bodies creates the same issue of burying drawing for P/N 456 inside drawing for P/N 123. I would then also have to send the entire drawing to the sheet metal vendor with an explanation to ignore this and that. "I" also would have to do that task. I couldn't use our ERP system and just order it because the folks that make all that happen are not in the engineering department. They would have ZERO sense that to find all the information for 456, just look in 123. They would have no sense of the "caveats" to explain to the vendor.
In a nut shell, more work up front, WAY less mistake later on. Pay me now or pay me more later....
As I said above, this process is NOT for everyone. But here it is for your review and maybe it will give you something to consider.