Assembly working directory

[Model_1975]

Hello,

I want to have a clear structure in my working area of CREO. Therefore I am working with folders where each part or construction group is sorted. For an assembly the single parts are sometimes in folders because of the overview and the structure. 

When I am loading an assembly it shows me missing parts. The path of those parts didn´t change.

Do I have to save every part of an assembly in the path of the assembly (and loose my structure) or is there a different way?

thanks in advance.

[Dale_Rosema]

When you say your paths didn't change, was the config.pro file update to include the paths that you have? If you start a new project in a new folder, that folder has to be added to the search path in your config.pro, else the software doesn't know where to look.

[Model_1975]

I introduced a new folder, where I am saving the assemblies as long as they are unfinished. After that I would copy the structure to our company folder / project folder. I am working locally because I don´t want to connect every time with our farm / servers. 

So I have to update the config.pro file or put all parts including the assembly into one folder or do I have to update the config file anyways? because for the parts which are in the same path like the assembly it´s working fine I think...Otherwise I have to update every project paths into the config.pro - this can´t be right?!

[BenLoosli]

If you read the documentation, you will see there is an option to use an external Search Path file.

In your config.pro, you put the location of your search path file and file name. By using the external file, you only need to modify the file and not your config.pro for any changes.

I am not positive on the syntax or name as I don't use search paths, but it something like this:

search_path_file c:\ptc_settings\search_path\search_path.txt

In your search_path.txt file, list each folder you want to have searched for your components, in the order you want them searched. The software will load the first match for a file that the assembly is looking for. This is critical if you use working and released folders for some of your parts.

[StephenW]

Creo doesn't "remember" file locations.

You can add search paths to your config.pro so it will look in specific folders you specify.

PTC has good documentation on this also.

https://www.ptc.com/en/support/article/CS20235?&language=en&posno=1&q=search%20path%20&source=search

[Model_1975]

Thanks Mr. Williams,

I only can see the general info from your link, not the details...only for maintenance...

Anyways - I can update the config file - can I search for it or is there one specific path for this file which I have to use?

[StephenW · Accepted solution]

Sorry the link wasn't helpful. The info is below.

I use PDMLink now so my help may be dated.

I would suggest you make a search path file (see below) for each project you are working on so you can only load the search paths for that specific project. The more search paths you have, the longer it takes for Creo to "look" for files. 

As far as the location of the config.pro file...that's gonna be specific to your organization. Usually there is one in the "text" folder in you creo installation. There may also be one in your startup folder (when you load creo from your icon, it's the working directory initially set before you change it). There may also be one in your "documents"  folder. Hopefully you have one that is designated for you to modify. You might need to talk to your cad admin or whoever takes care of your creo installations and setups

Applies To

• Creo Parametric 1.0 to 7.0
• Pro/ENGINEER and Creo Elements/Pro Wildfire to Wildfire 5.0

Description

• How to set up a search_path or search.pro file?
• Adding search paths to avoid being prompted to locate missing assembly parts on retrieval
• Error "Model <filename.part> is not in directory" when trying to open a drawing
• Search_path and search.pro files point to designated locations other than current working directory
• How to have format retrieved when opening drawing
• During model retrieval, the search is performed in the following areas in the order shown:
  • Creo Parametric session
  • Directory in which the top model is being retrieved
  • Active workspace or commonspace
  • Current Working Directory
  • Other search paths and folders

Resolution

• Add search paths using one of the following methods: 
  • Specify additional directory paths with the configuration option search_path
    • Wildfire 5.0 and previous: Select Tools > Options > Add
    • Creo Parametric: File > Options > Configuration Editor > Add
    • Add search_path option with value set to full path to the directory
  • Type the paths directly into the search.pro file and set the configuration file option search_path_file
    • Wildfire 5.0 and previous: Select Tools > Options > Add
    • Creo Parametric: File > Options > Configuration Editor > Add
    • Create file search.pro - see help file: To Edit a search.pro File
    • Add search_path_file option with full path to the search.pro file as value.  See help file: To Load a search.pro File

Note : If any of the directory paths specified in the search.pro file contains empty spaces in their directory names, enclose the whole path with in double quotations " "

Example: "D:\Creo Standard Parts\Bolts" --> As this path contains empty spaces, the whole path should be enclosed with in " " to make is read completely by Creo

[TomU]

Creo prefers to pull everything from one directory.  Yes, you can make it pull from other ones, but you will have to configure you Creo session to do so (with search paths) and anyone else you share that folder structure with will have to do the same thing to their Creo session.  Unless you have a consistent config shared with all your users, it might be easier to just keep everything in one folder.

[Model_1975]

Ok - so based on "I don´t want to change the config-file because I would have to do this for every project and after 30 projects I would have at least 30 new paths registered in this file and the loading time of creo would decrease with every new path...sometimes you have to look up old files" (otherwise data backups would make no sense). 

If so - ok, so far understood. I am working on a project where we have at least 12 parts for one assembly (which may be not that much compared to bigger assemblies) but so far I have of each part at least 1 saving so 2 files in my whole folder for creo files for this project. Some parts have up to 18 versions because of the adjustments which had to be made.

Is there any way to solve this mess or do I have to cope with a big list where every xth file has to be found to make sure I open the latest one?!

I could drag the older versions into a separate folder but I am not sure if creo likes this way of working...for example I have a part with 18 versions (.prt.18 is the latest one) Would there be any disadvantages to put all the .prt.x up to .prt.17 into another folder to tidy up?

thanks in advance. 

[Dale_Rosema]

Depending upon how long you need to save them there are purge utilities available to remove the older instances of the part. Creo always pull the latest (highest number from what it can figure out - not date) when loading files.

https://community.ptc.com/t5/System-Administration/Spekan-Purge-Utility/m-p/121135

https://community.ptc.com/t5/System-Administration/Spekan-Purge-Tool/m-p/415298

[KenFarley]

This kind of thing has been discussed before, the key phrase to find lots of information about it is "search path". Here's a discussion I responded to with a DOS batch file that builds me a complete local search path file when I have a large project that I've organized into tidy subdirectories.

Old Search Path Discussion 

That little batch file has saved me from a lot of trouble as some of our projects sprawl out into 20 or 30 directories and sub-directories.