Turning Parts into Assemblies, Assemblies into Parts (Part 2 & 3)
This is a series of blogs from me about turning Parts into Assemblies, and Assemblies into Parts in SolidWorks.
This blog (Part 2 & 3) will show you TWO ways to turn an ASSEMBLY INTO A PART.
Why would you ever want to do this ?
How about if you download an assembly from the internet or your customer or colleague gives you an assembly and all you care about having is a PART file. The PART file will be smaller in file size/details and will perform better.
Perhaps you want to send your assembly to someone else but first want to “lock it down” so there will be no feature tree so they can’t change it.
Maybe you don’t want to accidentally screw up some mates in the assembly, so making it a part would accomplish this too.
I’m sure there are other great reasons…
Here is how you do it.
1st way (NON-ASSOCIATIVE):
Simple as can be, but a lot of people would never even dream of trying it…
Open your assembly, do a SAVE AS, and change the “Save As Type” drop down box to PART.
There are some options that show up then asking what exactly you would like to be saved.
Just the Exterior Faces ? The Exterior Components ? Or All Components ?
Done, easy, finished…
This method is a “one shot deal” though. It is NON-ASSOCIATIVE.
i.e. the part WON’T UPDATE if the assembly is changed.
2nd way (ASSOCIATIVE):
If you want your resulting part to actually UPDATE if you ever make changes to the Assembly it is coming from, this is the method you need to use.
The command you will use is INSERT–FEATURES–JOIN.
However, when you are in an Assembly file you can not do an INSERT–FEATURES– anything…
So the first step is to make a NEW empty part IN the assembly.
INSERT–COMPONENT–NEW PART. Select a face or plane in the assembly that you want to be the FRONT face of the new part (doesn’t really matter for what we are doing). A “side-effect” of the Insert New Part command is that it puts you into a SKETCH on that face you selected. Usually this is great, but in this case we don’t need it, so just EXIT THE SKETCH.
Now you are in EDIT PART mode in the new part, and you CAN go to INSERT–FEATURES–JOIN.
Select the parts you would like to join together into your PART file (don’t have to select them all) and hit OK.
Now if you SAVE that new part, you will have what you wanted, an ASSEMBLY TURNED INTO A PART !
In that Part file there is an external reference (the “->” symbol in the tree) showing you that any changes in the Assembly WILL propagate down to the PART.
Furthermore, if you don’t want the resulting part to be a MULTI-BODY part, you could use our boolean COMBINE command and the ADD option.
Hope you can find some uses for this !
Let us know !