retrieve missing files

[fdefilippi]

I'm very confused and lost on PTC-Creo's file management.   I created an assembly yesterday, with files in different directories, this morning I restarted the program and it can't find the files, not only that but it doesn't tell me were they are located so I can retrieve them to reestablish the links..

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[StephenW]

There are no "links" for directory locations. Assemblies do not record directory locations of parts or sub-assemblies.

Per Doug Schaefer:

When opening an assy, Creo will look for the parts inside in the following places, in this order:

1. In memory (In Creo, closing a window does not close the part / assy / drawing / etc. from memory).
2. The folder the assy came from.
3. The current working directory.
4. Any defined search paths in your config file, in the order they are listed in the file.

Search paths can be defined in 2 ways.

1. use the config.pro option SEARCH_PATH followed by a directory path

2. use the config.pro option SEARCH_PATH_FILE followed by a search.pro file name. That text file contains directory paths of where you want Creo to look for files.

[fdefilippi]

Thanks Stephen,

One question, I have.  I replaced the previous engineer here, and when I open one of the assemblies he worked on not all the files are loaded.  So I spend a long time trying to find these files on the network.  If the files are not loading it doesn't tell me were to look, there is no point on what director this files is located, does Creo have some option to help locate files?   Sorry, still confusing on my end

[StephenW]

Creo really doesn't help locate files. About the most help it gives you is if there is a file that it can't find, it will allow you to browse tothe file yourself, but you have to know where the file is.

So my suggestion for you, look at the config.pro from the previous engineer and find the "search" options from the previous post. If there are search paths specified or search pat files specified, it is possible you are putting files in directories that are not specified in the search path. You would need to add your new paths so next time you open creo, it will know to look in those folders.

If your Creo files are in a lot of directories, you likely have a search path file that tells creo what all these directories are. Any new directories you add new, you will also need to add that path to your search path file. A search path file is simply a text file containing directory paths. See image below.

[fdefilippi]

Thanks again,

I'll look into this, still sound very confusing..

[StephenW]

So let's go basic.

1. Creo assemblies do NOT track where the parts are located.

2. When you open an assembly, the first place it looks for the parts is parts in memory (already opened parts). (see FILE - OPEN - IN SESSION)

3. If the parts are NOT in memory, the next place is in the directory that you are opening the assembly from.

4. If the parts are not there, then next place is current working directory (see FILE-OPEN-WORKING DIRECTORY)

5. If the parts are not there, then it goes through the search paths and search path files that are listed in the config.pro for your current open session of Creo.

[fdefilippi]

Thank you, something I will print out and hand on my wall.

Jus curious, what is the advantage of Creo not remember search paths and operating this way?

thanks again

[StephenW]

If the parts remember, you can never ever move the parts/sub-assemblies.

You have full control over where the parts/sub-assemblies come from, this gives you the ability to separate one project from another, if you need to, keeping all files separate.

It is really powerful and yet dangerous. If you end up with the same model in more than one location, you may have a huge problem.

[fdefilippi]

I agree with your first statement based on my SWX/ Inventor experiences, broken links are hard to fix, which is why a PDM system is used.

[StephenW]

I have been at jobs that use PDM for years now. Going back to manually managing the file locations and folder structure would be a shock to me too.

[fdefilippi]

that's what I'm doing now.   However I'm the only engineer here so not sure if PDM would be helpful.  I'm still trying to learn Creo 3.0 on my own.. 4 months later.. ugh

[dgschaefer]

For me, the advantage is having simple rules for where it looks is that I can feel free to implement whatever file storage system I want I can be sure of how Creo will look for the files and I can reliably predict what file it will find.  Keeping Creo a bit "dumb" in this regard gives me more flexibility to be in control of my files.  It actually forces me to be more disciplined with my files because I know it's on me.

If Creo keeps track internally where the files are, if I move one it'll be lost.  I also won't know what file it will find until after I open the assy and do some digging to see where it came from. If a save as operation puts a copy of a part in a new place with the assy opened and the assy gets saved, it may now be referencing the other version of that part and I may not catch it.

SW keeps track and it's bitten us in the past.  Specifically, when a part gets saved to a user's hard drive (because he took his laptop home to work on it, perhaps) but the assy is on the network.  Another user tries to open the assy and the part isn't available, even though the first user did put it back on the network, in the folder with the assy.  But because SW is trying to be smart, it actually gets in the way.

[BenLoosli]

UG/NX does store the file path of the components in its assembly file, but the load routine is smart enough to look in the search paths if it doesn't find the file where it thought it should be. Maybe a little more work for the programmers but saves a lot of headaches when a file is moved. We used to move UG/NX files from in-work to released folders with batch scripts, so the fact that they could still be found saved a lot of time.

When we moved to Pro/E in the 2000i/2001 release time, we put in Intralink because Pro/E did not keep track of files, plus you now had multiple file types to deal with. When we made the move to Wildfire2, we also migrated from Intralink to Windchill/PDMLink.

For one person, any PDM system would be expensive and over-kill. You just need to understand how Creo loads files and maintain the search.pro file. Remember that the search.pro file is only read at start-up time so any changes require a restart of Creo.

[fdefilippi]

Maybe for Creo a PDM would be overkill, but as a sole SWX user at my last place, a PDM was a must.   there was not version history

[dgschaefer]

That's the benefit of the Creo system.  With PDMLink it manages everything, without it manages nothing.  It makes working alone or in a small team feasible without a PDM system.  We routinely work in teams of 5-6 people on databases of 200+ objects without PDM.  That's probably pushing it, but it is still workable.