We’ve all been there at some point or another. We’ve all modified a part and maybe changed the name of it, and our references got all screwed up. Typically, we get a message to the effect of “SOLIDWORKS cannot find file Old Part.SLDPRT. Would you like to find it yourself?” to which you can reply Yes, No, or Cancel, with the option to not ask again. This only appears if you’ve renamed the part completely.
If you wanted to keep your old part, you might have saved a new part called “New Part” (which is, by the way, the worst name you can give to a part) and modified that, but were unlucky enough to not have had the drawing open when you did that.
This means the new name does not get reflected in the drawing, and the drawing (and assembly) still calls for the old part. A better workflow would have been to save the part as “Older Part” or “Old Part – CURRENT-DATE” using the Save As Copy option, then modify the part to keep it current, which would leave all your references intact. That will work great next time, but you’ve already gotten yourself into this mess and need to move forward.
Ideally you just want to change the part reference that the drawing or assembly is calling up.
Why change SOLIDWORKS Drawing reference?
Below is the existing drawing of the old part. I’ve got some dimensions on there, some GD&T, maybe it’s a more complex drawing that I don’t want to redo. Here’s how I change it.
Change reference steps
Firstly, I close the drawing.
Then, I go to open it again by going to File > Open (or use the Open icon on one of my toolbars).
While in the Open dialog, I’m going to pick the file, but I’m not going to click open just yet or double-click it to open it. Instead, I’m going to click on the References button.
That’s going to bring up a list of all the files that this drawing file is referencing. I could get the same list with my file open by going to File > Find References. This is what that window looks like:
If I double-click on the part (in the red circle) I can change the name of the part that the drawing is going to reference.
If I double-click the file path (blue circle) I can browse to a different folder. It’s generally good practice to keep your drawing files in the same folder as the part/assembly that it is referring to. That way, you can open the drawing by right-clicking on the part at the top of the feature tree and choose Open Drawing.
You’ll notice that changed items are listed as green. This is not permanent yet. This is not even permanent after I click OK. I have to click OK, then open the drawing for the changes to be applied, then I have to save the drawing for the changes to be made permanent.
In this example, since the new part was based on the old part, the dimensions are able to maintain their relationship with the correct edges and rework is minimal. Of course, if the part was completely different then I would likely need to create a new drawing anyways.
The same principle applies to an assembly as well. Mind you, in an assembly it is easier to right-click on the part in the feature tree, select the two chevrons at the bottom, then select “Replace Component” as shown below
As with replacing the reference component of a drawing, you also can end up with issues if the new part wasn’t based on the old part since the mates and sketch relations may be messed up, but if the new part was based on the old one then the issues should be minimal.
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