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Dividing one part file into many

srascha

New member
Hi All,


I am a sculptor using solidworks to visualize and produce a large wall-relief that will be fabricated using a cnc milling machine (small one - 300mm x 400mm). I was wondering if anyone knew of a way to section out a large part file (the relief which is 600mm x 2400mm) into smaller part files which I could then fabricate with the small milling machine and fit together afterwards.


The other way I am thinking is to just create the smaller separate parts files and then assemble them in solidworks to see what the whole thing would look like, but then I lose the ability to design the overall form (which is a large complex loft) with ease.


Any help would be greatly appreciated!


Thanks,


srascha
 
The easiest method is to cut your model using planes if you don't want any of your section pieces consumed by "saw cuts" or "flame cuts".

I LIKE to make some small welded assemblies using an alternative
method without the need for mates, yet can easily be edited. Our shop
doesn't like to see the welds shown so this works quite well.

The approach I use is to make a part with several bodies and then split the bodies up into their own separate files.


The way I like is when I make the initial model I intentionally make
each section piece where they don't merge together into each other.
This is accomplished by unchecking the "merge results" box as you
create and build up the solid model. What this does is create separate
"bodies" (solidworks expression) instead of one single huge part. Since there are
separate bodies then you can visually see your results with each body
having distinct seams. When you have everything where you like it, then
you just need to use the "split" feature command on your multi-bodied
part. All you have left is to individually name each body to create
separate files. This will create your parts and everything is where you
wanted it without putting it together like lego blocks like your
typical SolidWorks assembly.
 
Hi


I think the solution to your problem is the split feature(Insert->Feature->Split). Now you can obtain a multy body part and also you can save each body like a separate part. Also you can work on all the bodies with features that have scope on all bodies.


Nucu
 
Thanks Nucu and Ridein!
Your replies really helped...split is the key! And then I can drag them back
into an assembly as separate files...perfect, thanks!
-srascha
 
srascha,


If you click on the "split" in the feature tree, you can select "create assembly". this will create an assembly of your new split model/solids.
 
I think what you want is to turn your sculpture into a top down model and split each part up into specific welment parts.
 

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