Components & Assemblies cant find each other. 1

[NCCGRAD]

Hi All,

this is a quicky, in pro/e ill create multiple components and save them in seperate folders depending on what they are (contacts, plastics, screws...).

When i created the assembly, everything was nice and dandy no hiccups. But now when i try to open that assembly, it always comes back with the notice that it cant find the components. Is this becuase the assembly is saved in a different folder than the components?

~~Joe

 

[dgallup]

You need to add search_path options to your config.pro or load a search_path_file. Pro/E always looks first in the directory where a drawing or assy is retrieved from, second in the current working directory (if different) then in the directories defined by the search_path options in the order they are loaded. If none of those work then it asks you to manually find the file.

 

[slamdfullsize]

could you explain a little better with the search_path option and how to load it?

im kinda retarded when it comes to programming stuff and the config.pro is a mystery to me.

but i work at a company that just recently (2 years ago) got pro e and we have been wanting a way to save everything seperately according to what they are instead of one big folder with everything.

thank you for your help

 

[dgallup]

This has been posted about 1000 times but here goes.
Pro/E loads 3 config.pro files on startup and the user can load additional files at any time. The default ones are in the install_dir\text, user's home dir & initial working dir. THESE FILES DO NOT EXIST BY DEFAULT, you have to make them. They are just ascii text files. They can hold one or thousands of entries. You really need to use the Pro/E help system or the PTC website for all the myriad of options.

To add search_path settings just add lines like:

search_path C:\cad_dir\parts
search_path C:\cad_dir\assys

I ususally just use a text editor but you can edit the files while in Pro/E as well. Tools/options.

 

[loudman]

That will work if you only have a few directories to search through. A better option is the search_path_file option in the config.pro. We have several hundred folders and sub folders of projects and parts (legacy junk that still gets referenced), and adding all those to the config.pro is ugly.

Failry simple to create:
1. Open cmd window and run the command:

dir c:\working_directory /s /a:d /b > c:\pro\search.pro

where "c:\working directory" is the folder location that you have all your projects and parts and "c:\pro" is the location you want to keep your search file. (NOTE: the directory must exist that you are dumping the search.pro file into, this dos command will not create the directory for you.)

2. Edit your config pro to include the option search_path_file and browse to the search.pro file you created in step one.

This can be handy if set up in a batch file and placed on the network so that multiple user stations can point to a master search.pro.

 

[dgallup]

It is better to organize your data in such a way that you only need files from your working directory and 3 or 4 additional directories. If a given working directory needs some extra models then I add an entry in the config.pro in that directory. Adding every single possible subdirectory to your search_path will increase the time it takes Pro/E to find models, particularly if the majority of your models reside in directories at the end of the list. In our case, adding every subdirectory would create 477 directories for Pro/E to search. The first 237 of those contain ancient data that I have put into a directory called archive.