The assembly is too bulky can I make a block out of it so I can replicate it multiple times without freezing my computer
Try saving it out as a parasolid. The reinsert it.
When I open it after saving as parasolid SW converts it back to parts. I want one part that looks like the assembly
Ok, what if you were to suppress that part. Then export the assembly as the parasolid.
Import the parasolid, then insert that part into it then insert that into your assembly.
Does that make sense?
Where is the export option?
It is basically doing a file>save as>parasolid
I know of 2 general ways to go.
1) as Scott suggests, save it as a single file - parasolid, step, iges, etc. or even a sldprt.
pro - generally VERY large impact on performance.
con - new file is not associative to your original assembly - i.e. any changes to your original asembly, and you will need to do the save-as again and likley redo makes in the higher level assembly.
2) speedpack - makes a "light weight" derived configuration of the assembly
pro - since it is a derived configuration, remains largely associative to the original
cons - limits selection options in the upper level assembly to what is included in the speedpack
Message was edited by: Jeremy Feist
This is ridiculous, ill just make a rectangle to represent the assembly. Hope SW fix's this should be simple to convert an assembly to one solid part.
How About Saving the Assembly as a Part?
Switch SAVE AS TYPE to PART
Chose your option of Ext Faces, Ext Components or All Components and hit save, simple enough?
doesn’t work, saves as a part with 1000 individual pieces
Right, if you geomtery is line to line, then use the combine command within that part.
If you are just wanting to represent th Sub in a TLA you might try the other two options, and see which works best for you.
Additionally you can create a versions without Hardware (you know, that nasty, repetitve stuff that sllllllooooooowwsss down Assembly Re-Build Times) and save that as a part with only exterior components (getting rid of all those pieces that are nested inside another part, like bushings, bearings, snap rings, seals, etc...) and then do a combine feature on the remainder. Then you might try saving that sigle solid body part out as a para or step and import it back in to further reduce the part size.
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