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Unretrievable Models and Assemblies

asmith-3
1-Newbie

Unretrievable Models and Assemblies

Why is it that when working on an assembly or model and the window is closed or the computer gets turned off / restarted does Creo lose access to models, assemblies, and/or drawing?

 

I keep getting error messages that says the model or assembly cannot be retrieved. How do I re-associate them to the workspace I am working in or make the program be able to retrieve whatever I am working on?


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1 ACCEPTED SOLUTION

Accepted Solutions

Sounds like you might be a more experienced SolidWorks driver? SW and Creo have a fundamental difference in the methodology in the way it manages work flow data.

1. In Creo, data you are working will be "in Session" (I.E. in memory) and will keep that data "accessible". Even if it's not on the screen it will still be in session. If you "erase in session and/or not displayed" then that data is erased from memory, like it was never retrieved. This is the answer to your question "How would that change in a matter of minutes?

2. Creo has distinct control of where the data you are working on is retrieved from. Unlike SW where it goes and looks anywhere and everywhere for a file with the name it wants, Creo is specific as to the location of the file. You should set and work in your "working directory" and keep all the files there. However you do not have to. A "Search Path" in your config file will direct Creo where to look for the files you need. This the answer to your question Also, how do I fix this?

Below is what a search path line item looks like.

config1.jpg

View solution in original post

18 REPLIES 18

Search Paths in your config file.

How would that change in a matter of minutes?

Also, how do I fix this?

Creo does not keep track of where files are located unless you are using PDMLink for data management. You mentioned a workspace above, but I'm going to assume that you meant a Windows folder rather than a PDMLink workspace and that you are not using PDMLink.

When you open an assembly or a drawing, Creo looks for the parts & subassys that it needs in this order:

  1. In session / memory
  2. The folder the parent object came from
  3. The currently set working directory
  4. Any search paths defined in your config.pro file

The simplest way to make sure that Creo can find everything it needs is to keep everything in the same folder. If you have common parts, you can create search path entries in your config.pro file with this context:

search_path [full\path\to\folder]

You can create as many of these lines as you need.

Alternately, you can create a "search path file" (typically named "search.pro") with all those lines in it and then set your config.pro file to use it with this setting:

search_path_file [full\path\to\file]


I hope that helps,

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

Sounds like you might be a more experienced SolidWorks driver? SW and Creo have a fundamental difference in the methodology in the way it manages work flow data.

1. In Creo, data you are working will be "in Session" (I.E. in memory) and will keep that data "accessible". Even if it's not on the screen it will still be in session. If you "erase in session and/or not displayed" then that data is erased from memory, like it was never retrieved. This is the answer to your question "How would that change in a matter of minutes?

2. Creo has distinct control of where the data you are working on is retrieved from. Unlike SW where it goes and looks anywhere and everywhere for a file with the name it wants, Creo is specific as to the location of the file. You should set and work in your "working directory" and keep all the files there. However you do not have to. A "Search Path" in your config file will direct Creo where to look for the files you need. This the answer to your question Also, how do I fix this?

Below is what a search path line item looks like.

config1.jpg

Ok, now two things.

First I want to thank you for your help as this is helpful to me.

Second is another question, we use Windchill and the workspace's we work out of should have an automatic search path and working directory set up. this is why this situation has me perplexed. For the most part this doesn't happen but every so often this situation arises. Now for the question, how with the search path and working directory preset, do I A) prevent this situation from happening and B) get the models to be retrievable once this happens and the model or drawing will not open?

Again, thanks for the help.

So you are using Windchill (PDMLink, I assume?), interesting. I don't have any direct experience with Windchill (but we are likely going to implement it soon), so my help ends here. I would have thought that PDMLink would have kept track of everything.

Sorry I can't help more.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn
BenLoosli
23-Emerald II
(To:asmith-3)

Once you start using Windchill PDMLink, the seach paths option is removed, it is not used by Windchill. Windchill tracks all of your files and knows where they are located at when it goes to retrieve an assembly.

This is one config.pro settings that will enable Creo to always utilize your Windchill data.

dm_remember_server yes

Are you renaming parts in common space, not that that should matter, but if you are getting disconnected from Windchill by your Creo sessions, it could.

When working with Windchill data, are your users disconnecting from Windchill manually for any reason? I have had some users do this and it messes them up badly.

I don't work offline, and the dm_remember_server is preset to yes

Are you using Windows WorkGroup Manager or are you pulling the "required" files when you retrieve into your workspace?

Couple thoughts on the PDMLink angle. If you retrieve required models, whatever is suppressed in model may not be retrieved. When you resume them it would grab them from the vault. If for some reason you lost connection to PDMLink and you were working "offline" it would not be able to retrieve anything not in your wo

I am using windchill to directly pull them into my workspace.

The most recent portion of this issue happened today. I had a sub assembly that couldn't retrieve a part so I removed the un-retrievable part from the the sub assembly and saved it. When I went to open the main assembly ( that I had up earlier today) Creo tells me that the main assembly is un-retrievable.

StephenW
23-Emerald II
(To:asmith-3)

Can you open the un-retrievable part by itself (not as part of the assembly)? If not, you may have a corrupt part. The part could possibly be corrupt in your workspace and otherwise okay. You may need to re-download the part. Just a thought.

For the most part the parts are newer and never checked into Winchill.

Are you using more than one version of Creo? Could it have been saved in a newer version of Creo and you are now retrieving in an older version?

No, I have been using Creo 2.0 and this has happened to me a couple times. I am getting tired of it happening and now trying to get to the root of the problem so that it will not happen again. Time is money you know, and this is a big time waster as I have been having to redo quite a bit when it happens.

AJ,

I have not had a corrupted model in over ten years so I would be really surprised if it turned out to be that. With Windchill all bets are off because it's such a cluster to begin with that it makes it very difficult to isolate what it is. If you have parts from a central library (fasteners, tape, labels etc...) that your assembly is drawing from then you might look at that. Especially if someone have revised anything while you have had the assembly in session.

I would try is pulling the last known good version of the data out of Windchill and getting it off the server. Save it, change it, save it again. Erase everything from memory, open it and then save it again. Try to find out if it's Windchill related or Creo related.

Have you used good modeling techniques? No flame intended but there can be references that get jumbled between parts if you have used a Top Down methodology and cross-referenced things. Do you find the assembly seems to take a long time to regen? Meaning if you edit a value in one part, does Creo seem to go and regen everything in the assembly? Do you have family tables (instances) in any of the parts? Have you referenced an edge, axis, surface, etc...from a part that is an instance in another part(s)? Do you have any articulating parts/features in the assembly that would make a reference disappear in certain configurations? Do you have different accuracies in your parts or assemblies and'or features that are dependent on relative accuracies for their regen success?

I am asking some far reaching questions because if it's one thing I know about Pro (A.K.A Creo) is the answer can be found.


StephenW
23-Emerald II
(To:DeanLong)

Every once in a while with PDMLink, I get a model (part or assembly) that corrupts in the workspace. I was just helping a coworker with one last week. Once you re-add the model from the commonspace, the problem goes away. Last weeks problem was a part that didn't even show as modified in the workspace but wouldn't open.

Are you doing any renaming from within Creo (not PDMLink)? The last time it happened, do you remember what operations you were doing prior to the failures?

Since you mentioned parts were new in the workspace, do you get any errors during saves sometimes that tell you something hasn't been saved? Occasionally with PDMLink, it'll throw an error and won't save. It doesn't do a good job of making this obvious. It's in the message log, "xxx.asm has not been saved". For us, these errors are usually associated with family table issues and occasionally library part issues.

Like Dean said, the questions are getting far reaching.


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