[ptcuser] - Can't get co-worker latest models

[ArnoldCollett]

Sounds like you are using a search.pro that is looking in the folder
with the old files. Try moving the old files to a backup folder.

Hope this helps,
Arnold

[dgschaefer]

I think the order of part retrieval is:
1. In session
2. folder the assy came from (if opened from a different folder
than the working directory)
3. working directory
4. search paths, in order
That's different from the old days where 2 and 3 were reversed. That
change happened in WF1 or WF2, I believe.

I honestly have no idea why PTC changed it, it messes me up all the
time. There's a config option that forces the old behavior, I think,
but I'm not sure what it is. I'm trying to get used to the new default
as it does make a bit more sense to pull the parts from the remote
folder if the assy is in the remote folder.
Doug Schaefer

[byork]

Unless you use the config option.





use_2001_search_order yes




Solution Details - TAN

Solution

130928

Type

TAN

Created Date

20-Oct-2005

Last Updated

30-Jan-2006

Title

When Retrieving Assemblies or Drawings in Pro/ENGINEER Wildfire,
Pro/ENGINEER Searches for Components in the Directory From Which the
File was Retrieved Prior to the Working Directory.

Details


Description


When retrieving assemblies or drawings in Pro/ENGINEER Wildfire,
Pro/ENGINEER searches for components in the directory from which the
file was retrieved prior to the working directory.

This behavior is different than specified in the Pro/ENGINEER help
document "Retrieving Files from Other Directories", which indicates the
search order is:
1. In session (in memory)
2. Current working directory
3. Directory containing the assembly or drawing file
4. Directories in the search path


Resolution


In Pro/ENGINEER Wildfire the search order is:
1. In session (in memory)
2. Directory containing the assembly or drawing file
3. Active Windchill or Pro/INTRALINK Workspace and Commonspace
4. Current working directory
5. Directories in the search path

The change was made in Pro/ENGINEER Wildfire, datecode 2002020 onwards,
through an internal development project which dealt with retrieving
objects into Pro/ENGINEER from Windchill and Pro/INTRALINK. It was done
to try to avoid opening some objects from local disk and others from the
PDM system. This change was intentional in accordance with Pro/ENGINEER
Wildfire behavior with Windchill and Pro/INTRALINK.

The Help Center document will be updated in a future version of
Pro/ENGINEER.


Alternate Technique


The original behavior can be restored by setting the hidden config.pro
option "use_2001_search_order" to "yes".