Solidworks 2014 - Convert a complex assembly into a single “inert” geometry file and import it

Question

I have a large and unwieldy Solidworks assembly and I would like to save it as an "inert" geometry file such as an STL or STEP format. Then I want to import this into another project assembly and move it into a specific location.

It seems that I am unable to move the STL version from its default insertion point in the new project. I have tried opening the STL file and saving it as a SLDPRT file and bringing this into the assembly but I am unable to move that either.

The reason I want to do this is so that there are no dependency links between one project and the other, in order to avoid any possibility of design corruption while I'm experimenting with the new assembly.

In a nutshell, how can I import and position an inert STL (or STEP or whatever) into an existing SLDASM file and be able to move it around?

Answer 1

In order to insert a 'dumb' copy of an assembly into another higher level assembly, you can save the assembly as a .SLDPRT File. Make sure to select the correct amount of geometry to save, according to your needs from the options in the 'Save As' dialogue.

This .SLDPRT will be completely independent from the original assembly, being made up of internally saved .IGES components.

You can then simply insert this new part into your high level assembly, and mate it as normal.

N.B., if you ever use the 'Edit Component' Function inside the Assembly environment, you can toggle "No External References", which will prevent you from accidentally creating references to the 'dumb assembly', e.g. by accidentally snapping a sketch point to it.

Answer 2

EDIT: I misread your question, and the below instructions are for inserting into an existing .SLDPRT file, not a .SLDASM file as requested - I'm leaving it visible for reference, as I believe the information is still useful. I have submitted a separate answer to your actual question!

When you insert the part (Insert --> Part), you can either check the box labelled "Locate part with Move/Copy feature", or simply use the Move/Copy Bodies Tool (Insert --> Surface --> Move/Copy) to move the object afterwards.

You can also choose to break the link to the part that you inserted at this point, so for a .SLDPRT file, you don't need to do any conversion. For assemblies, you will need to save as a .SLDPRT.

Make sure you select "All Components" while saving, if you want all the data to be present.

Once in the Move/Copy Tool, you can click the "Constraints" button to get a rudimentary version of the Assembly Constraints environment, but, I'd stick to translation where possible, since this then will not be affected by geometry changes, giving fewer errors.