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documenting an assembly in creo3

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documenting an assembly in creo3

Hi

I have a problem about saving and documenting an assembly in creo3.

I have three different machines that I want to save all of three assembly's files in one folder called "A". Also I want to save all parts of these assemblies in another folder called "B". It should be noted that some of parts have been used in all three assemblies. All of these parts and assemblies should have drawings that these drawings must be saved in another folder called "C".

My problem is when I put my assemblies in folder "A", my parts in folder "B" and my drawing in folder "C" and then close the Pro-engineering program after I open the program again all of the address links for assemblies and drawing have been erased.

How can I fix this problem?

Best Regards

Sattar Dagahi

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4 REPLIES 4

Re: documenting an assembly in creo3

Creo does not save folder locations (or address links as you refer to them) with parts or assemblies.

You need to set up search paths in the config.pro options file.

Please review the link.

https://support.ptc.com/appserver/cs/view/solution.jsp?n=CS20235&art_lang=en&posno=1&q=search%20path...

Re: documenting an assembly in creo3

I'd recomend putting all of your files in one folder.  You can set up search paths, like Stephen said, but there's no real advantage inside Creo to having them separate.  I guess it makes working with the files through windows easier, but again there's not a lot of value in working with Creo files directly through Windows, in my experience, excedpt for fining a file to attach to an email or soemthing like that.

--
Doug Schaefer | Engineering Manager
Crow Works

Re: documenting an assembly in creo3

I agree with @dgschaefer on the concept of keeping all your files in one folder unless you are working with 1000's and 1000's of files.

Re: documenting an assembly in creo3

We tend to keep all the pertinent files in one directory, too.

However, there have been some really large assemblies we've had to deal with that use lots and lots of springs, custom pins, complex sub-assemblies, etc. It got to be a real ordeal to find the file you wanted to open, especially if you kind of knew the name but not exactly, etc. So, I put the models, drawings, etc. in their own directories, grouped according to a logical method (Purchased Parts, Common Components, etc.) Since the project was constantly in development, I wanted to have the directory structure traversed and a search file built without me doing it manually. This way I avoided the inevitable spelling screw-ups, or missing a directory, etc. I wrote a batch file that did all the work for me.

Here's the Batch file code, just paste it into a batch file (*.bat) of your choosing.

::
:: Builds a "search.pro" file with a listing of all the subdirectories of
:: the current directory.
::
:: Author: Kenneth J. Farley
:: Date:   10 February 2015
::

@ECHO OFF

::
:: Build the local search path file so it reflects the current directory
:: structure. This will overwrite any existing file.
::

ECHO. >NUL 2> locsrch.pro
call :doPath "%CD%"
FOR /R /D %%d IN ("*") DO call :doPath "%%d"

::
:: Build the config file with the current date and the one search path setting.
::

ECHO ! > locconfg.pro
ECHO ! Local version of config.pro, built automatically. Load >> locconfg.pro
ECHO ! this file into your Creo session via the following: >> locconfg.pro
ECHO !     File-^>Options-^>Configuration Editor-^>Import/Export >> locconfg.pro
ECHO ! >> locconfg.pro
ECHO ! Author : %username% >> locconfg.pro
ECHO ! Date :   %date% >> locconfg.pro
ECHO ! >> locconfg.pro
set dirName="%CD%"
set "mapName=%dirName:~1,2%"
set "dirName=%dirName:~3,-1%"
for /f "tokens=3" %%a in ('net use %mapName% ^| Find "Remote name"') do set uncPath=%%a
set "absName=%uncPath%%dirName%"
ECHO search_path_file %absName%\locsrch.pro >> locconfg.pro
exit /b

::
:: Routine to convert a mapped directory to its UNC equivalent.
::

:doPath
set "dirName=%1"
set "mapName=%dirName:~1,2%"
set "dirName=%dirName:~3,-1%"
for /f "tokens=3" %%a in ('net use %mapName% ^| Find "Remote name"') do set uncPath=%%a
set "absName=%uncPath%%dirName%"
ECHO "%absName%" >> locsrch.pro
exit /b

How to use this?

(1) Put the batch file in the topmost directory of your project.

(2) Run it.

(3) Start up Creo as usual, then change working directory to the topmost one of your project.

(4) Load the "locconfg.pro" file via FIle -> Options -> Configuration Editor -> Import/Export

Now Creo will "see" all your files. If you make changes to the directory structure, just run the batch file again and it will overwrite the old files with the corrected ones.