The main premise is this; I would like to maintain a parametric bond with one part to another. If I change 1 part I would like it to be able to update the other.
I tried a new technique where I have the frame of the imported model brought over as a Copy Geom. From this imported surface frame I am using a referenced sketch which drives other details within the main model.
Everything worked great.
Then I moved the model that spawned the Copy Geom to another folder. I thought things were good until I went through the history of the main model and the referenced sketch had failures.
I believe the failures were because the main model no longer sees the imported Copy Geom model.
Is there a way to maintain the link between the main model and the imported Copy Geom model if they are in separate folders?
We don't have Windchill if that would allow the permanent linkage. I would like to know if there is any way of maintaining an external folder part link within base Creo, but if it isn't possible would Windchill allow this?
I seem to remember wanting to do this exact thing years ago. If my memory serves me right i used the config option search_path_file which points at a search.pro file which is a list of working directories. Its worth a try.
The search_path_file does sound like it could work.
I am wondering how you might add a folder to this directory?
I am also wondering whether this means that specific folder would be globally available for linkage if I opened up any model file or if the link would be local to just the model file that needs it (as I would prefer in this instance)?
Ben: Perhaps I'm not understanding this correctly but it looks like I may have already had search_path_file already enabled in config.pro. Possibly this may have been for a similar need I once ran into with assembly years ago.
It doesn't appear that any outside folders link up with files that I have worked with.
My temporary work around is to store all the files in the same folder but perhaps it can be explained how the linking can be possible.
Parts or assemblies don't maintain any path or folder location information.
The only way you can add folder location information is thru the search path or search path file option in the config.pro.
Every time you open an assembly, if the part or assembly is not in the working directory, creo will search the path's specified for the files.
At a past company, we had search paths for libraries that everyone used. We also had search paths for projects. If I was working on a forklift project, I would load the forklift search paths. If is was working on construction equipment, I would load that search path. If i was working on a contract manufacturing job, we would make a search path for that specific contract.
None of these files (other than library files) were intermixed. The directory structures could be as easy or complicated as you desire.
Don't forget that once you load the search path into the config.pro file, you have to reload the config.pro. There may be other ways to do this, but I find that rebooting Creo works the best.
Windchill would maintain the link as it knows where all the files are within the system and any moved files will get their link updated.
Outside of Windchill, the search path option should load your file after it has moved and you have updated the search paths. You can either use Search_path in config.pro or Search_path_file and point to a search path file. I find using the file for your search paths is easier to maintain as you don't have to update config.pro everytime you need to change your search paths.