Do you have external references in your SOLIDWORKS file that you need to manually remove? Then this article is for you! Refer to other posts at the end of this article to learn more about what external references are and when they are appropriate for use. The scope of this piece will be purely about manually removing external references in part files.
Looking at the assembly FeatureManager Design Tree, we can identify the external references by the external reference symbols on the components:
In this example, I will take the Jaw_Plate component and remove external references. I want to use Jaw_Plate in other files/assemblies, so I must remove any and all external references so the file is self-sufficient.
Upon opening the file, I can see what features have external references by looking for the external references symbols:
By editing the sketch (1), we can see Convert Entities relationships on all sketch entities (2). By using the Display/Delete Relations (3) command and setting the selection to External (4), we can see a list of all external references (5):
To remove all of the external references, I'll use the Delete All command (6). I'm now left with a sketch with no relations or dimensions:
It’s always good to have a sketch entity tied to the origin, so I'll use the Move Entities command to move my entire sketch as a block:
After some cleanup (in my example, I have three collinear lines on the bottom of the plate from the Converting Entities command, so I'll delete two and extend one to complete the profile), this is where the magic happens. Now that the sketch is in place, use the tool Fully Define Sketch:
This tool will be used to automatically add relations and dimensions defined exactly how you want them. The original sketch geometry and shape are perfectly maintained using this tool.
In my example, I will add all relations possible (1), set my baselines to the origin (because it is now at the bottom-left corner of my sketch) (2), and click Calculate (3):
The wonderful thing about this tool is that they are not permanent. If you wish to not include certain relations or change the behavior of your dimensions (Ordinate, Baseline, Chain), you can simply make the change and then click Calculate again. Only once you are happy with what you see is it time to click the green checkmark to accept the definitions.
Exit the sketch, and we’re done (at least with this example)!
We now have a component that is completely independent of the assembly and can be used wherever we like. We can also sleep easy knowing that the geometry of the file is exactly as it was defined in the assembly.
I hope you found this helpful! Check out the links below to learn more about SOLIDWORKS references.
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