In Wednesday’s competition we learned neither our champion nor challenger’s method of updating references worked. Did you figure out why?

The problem they ran into was caused by how SolidWorks finds referenced files when assemblies are opened.

SolidWorks has a set of rules to go by when trying to find components of an assembly. It is important to know and understand SolidWorks’ method.

1. Try to use an already loaded file
2. Look in the paths listed in the “Referenced Documents” list in the options area
3. Look in the same directory as the assembly
4. Look in the directories where it has already found other components
5. Look where the file was the last time the assembly was saved (excluding the drive letter)
6. Look where the file was the last time the assembly was saved (including the drive letter)
7. Ask you where the file is

Both contestants correctly told SolidWorks to look in the new location, but SolidWorks would rather find the file within the same directory as the assembly was found. (Priority #3) It only appeared the references were not updated.

If either of our contestants would have deleted the motor from the assembly’s directory they would have won the autographed coloring book because SolidWorks would have gotten to priority #5 and the correct motor file would have been opened.

What is the moral of the story?

1. Spend some time learning how SolidWorks resolves referenced documents. This is a very important skill, that I promise can save you many headaches when files are acting funny
2. Never duplicate file names for SolidWorks files. If these two files would not have had the same name, at worst our contestants would have been notified that SolidWorks could not find the file (gotten to priority #7) and they could have known to fix the issue.

Welcome everyone to America’s favorite game show: “Why won’t these references update?!” I’m your favorite game show host Guy Smiley.

Today we have two challengers. Our first challenger enjoys hopscotch and talking to her gold fish, say hello to Penelope Pendelton!

Our second player enjoys working in his store, Mr. Hooper.

Here is the challenge: Today we received a set of files from an outside contractor. Our producers have copied the files from our ftp site and have added them to our network as shown here:

The challenge we have for the two of you today is that the “182T.SLDPRT” file is a standard product of our company and we wish for you to change the assembly’s reference to no longer load the file from this downloaded directory, but to use the file in our standard parts library instead:

The winner of today’s challenge receives a coloring book autographed by me, Guy Smiley.

On your mark, get set, go!

Our challenger, Penelope wastes no time opening SolidWorks and changing the reference through the “Reference” button in SolidWorks’ Open dialog box.

She quickly opens and saves the assembly and clicks her buzzer. 37 seconds, an unbelievable time.

Now it is our champion, Mr. Looper’s turn.

“Hooper!”

Mr. Hooper notices the assembly is stored in SolidWorks Enterprise PDM, so he uses EPDM’s “Update Reference” tool to change the reference in only twenty seconds!

It looks like Mr. Snooper has easily won this challenge, but let’s wait for the judge’s final decision.

Our judges go to each challenger’s computer, open each assembly and find the assemblies are still referencing the original motor! Neither method worked! Are we doomed to never have this assembly reference the file from the library like we want?

Both assemblies were checked out, the assembly files have a new time date stamp …what happened?

Tune in tomorrow to learn: “Why won’t these references update?!”

(Hint: This is not an EPDM issue.)