While in the drawing select the view from the design tree and right click, then select "Replace Model".
On the left a menu will appear. In this menu, under New Model, select Browse.
A file explorer will pop up and you should be able to browse to wherever your model is saved. Select the model you want the drawing to reference and select Open. Then, select the green check on the menu on the left hand side of your screen. Just a reminder, make sure that the file type drop down menu (bottom right corner) is set to either assembly or part, depending on which one you're looking for.
Now that you know how to do it, I will admit that it is a clumsy method. I am not sure why SolidWorks has not come up with a more straightforward method for this, such as being able to edit the path from the properties menu.
One way you may avoid this in the future is to use the Pack and Go feature in Solidworks. This becomes an invaluable tool when moving around assemblies. Imagine doing the steps above for a 500 part assembly.
Possibly easier to use SolidWorks Explorer, a powerful tool to control many variables outside of SWx.
Navigate to the drawing in question, click over to the references tab, and replace with desired model.
In the future, when moving files, it's a good practice to right click on the file, open the SOLIDWORKS flyout, then click move. That will relocate your reference links as you move files.
An even easier method to update the reference of the drawing on C:\ drive is to close all files, then open 'a.sldprt' from the new C:\workingfolder directory. When you open a drawing or assembly that references "a.sldprt" it will first look to any files already open in memory with the same name. So then opening the drawing from C:\workingdirectory will now reference the 'a.sldprt' from C:\workingfolder and you can Save to keep this updated.
Another approach to see all references at the same time is to go to File > Open in SOLIDWORKS, highlight the local drawing file, then click on the 'References..' button in the bottom left. This will list all references and you can double-click on any bad references to browse to the correct file.
But as John mentioned, try to use Pack and Go from the assembly in the future as it automatically updates the references in the copied files. There are a lot of useful features in Pack and Go as well.
Or consider implementing PDM to have references update immediately when renaming and moving directly within Windows Explorer.
I agree with Scott Durksen. If you'll open the Part from the working folder first, then the Drawing, the Drawing should reference the open Part. When you save the Drawing it should save the new reference.
I didn't realize that I had the same question, but apparently I have been going about this the wrong way. I typically turn to pack and go for large assemblies, but I think I will begin taking Scott's advice from now on for individual parts. I always thought that it was a little unpredictable, but that was probably because I was not consistently opening the model first. Good to know! Thanks.
There's nothing wrong with Pack and Go. I use it frequently myself. If Gianfranco had done that instead of just copying the files then he wouldn't have (or at least shouldn't have) had the problem. The solution I posted above was for dealing with the situation he already has. It wasn't intended to be a recommended practice for the future.
I knew what you guys were talking about, but I think I could have done a better job clearly typing out my reply to Scott. I meant that I have always (and will always) turn to Pack and Go for large assemblies as it is a little more automatic for multiple parts/assemblies. But I didn't realize there was an easier secondary method. And actually, now that I know what it is, I would almost argue it is easier than Pack and Go if dealing with an individual file. However, I do wish that the file path could be edited in the properties window.
In general, you should always avoid having multiple copies of the same file name. Otherwise if you have 'a.sldprt' in multiple locations, you may inadvertently have the wrong 'a.sldprt' open in the background and have your drawing change reference. Better to Pack and Go and add a suffix or prefix if it's a new project (i.e. 'a_rev2.sldprt').
Thanks to everyone for all the good suggestions.