Hi Kris...
There's a specific order Creo (or Pro/E) uses to look for models upon retrieval:
- Models already loaded into memory ("In Session")
- The directory where the drawing is being loaded from. For example, with you selectthe File Open command, you can navigate to other folder to open files. If you navigate to some other folder, this "other folder" is searched.
- Active Windchill or Pro/INTRALINK areas:
- Workspace
- Commonspace
- Your Current Working Directory
- Search Paths defined in your config.pro and/or paths in the Search Path File defined in config.pro
What's happening here is that you need to set up your search paths. Working without Windchill or Pro/INTRALINK (also called "Wild West" style) can be tricky. Often you maintain a list of search paths to instruct Pro/ENGINEER where to look for files. For example, if you decide to put common hardware or purchased vendor items in a special folder somewhere, you'll want to add that folder to your search paths.
Search paths can be added in two ways. First, you can open up your config.pro file and add lines to it. If I recall correctly, you're running Creo Elements Pro/ 5.0. From your top menu, you can also edit your config.pro from the top menu by going to to Tools->Options. You'll add lines like this for each folder you want the system to search:
search_path "<path here>"
For example, you could add these lines to your config.pro:
search_path "c:\documents and settings\username\my documents\vendor_parts"
search_path "c:\documents and settings\username\my documents\hardware_library"
search_path "c:\documents and settings\username\my documents\hardware_library\screws"
search_path "c:\documents and settings\username\my documents\hardware_library\nuts"
search_path "c:\documents and settings\username\my documents\hardware_library\washers"
search_path "c:\documents and settings\username\my documents\hardware_library\bolts"
Instead of specifying them line-by-line in the config.pro, you can put these pathnames into one text file and reference it using the search_path_file option. Instead of multiple "search_path" statements, you just have one search_path_file statement in this format:
search_path_file "<path here>\search.pro"
For example, you could add this one line to your config.pro:
search_path_file "c:\documents and settings\username\my documents\search.pro"
Then you could have a search.pro file with these entries:
"c:\documents and settings\username\my documents\vendor_parts"
"c:\documents and settings\username\my documents\hardware_library"
"c:\documents and settings\username\my documents\hardware_library\screws"
"c:\documents and settings\username\my documents\hardware_library\nuts"
"c:\documents and settings\username\my documents\hardware_library\washers"
"c:\documents and settings\username\my documents\hardware_library\bolts"
I understand going through this process might seem hard to justify, but there is a reason. Working without Windchill, sometimes designers will work on multiple projects. You can have a different set of search paths for different projects. This restricts Pro/ENGINEER's search capabilties to certain folders rather than have it search all over the place for files.
One final note... another technique you can use is to load the model into your session memory before opening the drawing. Once you've opened the model, Pro/E will open the drawing without a problem because you're using that #1 search location from the list above.
Setting up search paths is the way to solve your problem. If this email hasn't given you enough information, you can go to the help files and search for "search_path". You'll get much more complete information there.
Thanks!
-Brian
