SOLIDWORKS 2019: Saving an Assembly as a Part
What's New in SOLIDWORKS 2019
‘Saving an Assembly as a Part’ is another great new feature of SOLIDWORKS 2019. Simple but powerful. SOLIDWORKS has updated the ‘Save As’ option for when you Save an assembly as a SOLIDWORKS part file (.sldprt).
Some of you may not have been aware that you could even do this, but this option has been around for a long time. It’s a useful workflow if you have a complex assembly that you want to simplify. The assembly can either be something that you created yourself or that you have received from an external source.
There are usually 3 main goals:
- To make your top-level assembly lighter
- To send your assembly out to an outside vendor as a place holder in their larger top-level assembly
- You are wanting to protect your intellectual property by removing a lot of detail of the internal workings of you assembly, hiding certain pieces that are either not done yet or you don’t want them to see.
In the past you would do a ‘Save As’ on your assembly as a SOLIDWORKS part file (.sldprt), then open the new part file, use Delete Body Feature(s) to remove all the internal/other parts you didn’t want anyone outside the company to see. Next, save the part file as a Parasolid (.x_t) or another generic 3D CAD format. Finally, you would send the generic 3D CAD format or reopen the Parasolid back into SOLIDWORKS and save again as a part file (.sldprt)
AND.... the above process was a ONE-SHOT DEAL. If you needed another one you would have to go through the process again.
Now that whole process is magnitudes simpler.
With the new ‘Save As’ options for SOLIDWORKS parts, we just set which parts we don’t want to get saved out and then... ‘Save As’ > set the ‘Save as type’ to Part (.sldprt) > select the option to ‘Include specified components’ and hit the ‘Save’ button. DONE.
Here is a look at the 2019 ‘Save As' window. You will see that they moved the ‘All components’ up to the top. The ‘Exterior Faces’ is still available, but ‘Exterior components’ has been replaced with ‘Include specified components'.
Here is a screen capture of the 2018 ‘Save As’ window just for comparison.
How to Use:
How do you set the ‘Specified Components’ that you want to include? For this, we go into the Component Properties of the part or sub-assembly.
Hint: I found that you could use ctrl + <selection> or Shift + <select> methods to select multiple part(s), sub-assemblies or a combination of both, to change them all in one shot.
You can then either left-click or right-click to get to the Component Properties icon.
Once in the Component Properties window, you’ll see a new section called ‘Save assembly as part’.
When you have multiple components selected and you change them to ‘Always exclude’ and click the ‘OK’ button, they are all set at the same time.
Then we’ll go to the File Menu > Save As, select the ‘Save as type’ to be SOLIDWORKS part (.sldprt), then select ‘Include specified components’, and click the ‘Save’ button. It’s that easy.
But wait there is more...
There is whole new section in the System Options that can be used with the ‘Save As’ to customize this new functionality.
Click Tools > Options > System Options > Export. Then set the ‘File Format’ to ‘SLDPRT from assembly’. These options are used when your Component Properties for your parts and sub-assemblies is set to ‘Use System Settings’.
- ‘Visibility threshold’ is for auto-removal of internal parts. The greatness of this functionality is that if you have PCB or something similar, on the inside of a housing and you want a quick way to remove all the tiny surface mount components, this would be great for that.
- ‘Bounding Box Volume less than’ option is for the removal of components that are below where the volume threshold is set at.
- This one took me a little bit longer to come up with a good use for, but I could see if you had a much larger assembly that you were trying to save as a part that is simplified, then I could see this option of some use.
- ‘Fastener Components’ is for any part that has had the ‘IsFastener’ property set to 1. i.e. Any SOLIDWORKS toolbox part or any part that you have the ‘sldsetdocprop.exe’ ran on them or they came from SOLIDWORKS with it already turned on.
- Again, a great feature for quickly removing a bunch of toolbox parts from a large assembly that you only need to use as a place holder in your top-level assembly.
Happy Saving As part.