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Assembly Backup replaces modified components in WIP - Creo

ptc-6081577
1-Newbie

Assembly Backup replaces modified components in WIP - Creo

I received a part from a department a month ago. I modified it and created a new drawing and kept it in my local directory.

Now they have sent me an assembly which uses their original part. Now I set my local directory as working directory where I have my modified component and backup their assembly into my local directory. This is where the problem begins. Creo brings the unmodified part into my directory and replaces the modified part for which I have created drawing.

In ProE, The same procedure brings the assembly into my directory but keeps all other parts as it is in the working directory. This keeps my drawing intact. I want Creo to behave in this manner. Is there any config.pro option for that?

Thanks…


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1 ACCEPTED SOLUTION

Accepted Solutions

I found an old internal PTC document about the change, which named the option Doug remembered. Ganesh, you may want to test with the hidden config.pro option "use_2001_search_order yes" (it still exists in Creo 2.0). But keep in mind that you have changed the default order, in case you get unexpected retrieval results at some point. After all the change to the order had been done intentionally, to avoid situations where you retrieve an assembly that has all components stored and end up with some components being loaded from the current directory instead. With this in place, when modifying and saving the assembly, some changes may be saved to a different directory than expected (the one that was current when retrieving). With the new method you can still replace components with those from current directory by opening them into session first, but it cannot happen unknowingly anymore. Gunter

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14 REPLIES 14

I think you may have opened the assembly with the old part before you made the local folder your working folder. it would overwrite your newer part in this case.

Hi, Thanks for the reply. I have set the "working directory" before opening the assembly. Here is what I have done.

1. Set working directory where I have the modified part.

2. Open the modified part with the drawing and confirmed that it is good.

3. Cleared memory (Erase not displayed)

4. Click open, go to the other folder and open the assembly.

5. Save a backup in working directory (i.e current folder).

Thanks.

I think it is in #4. that the problem comes in. I often find that my "working folder" changes magically when I navigate to other folders, even in some very unrelated thing like picking up a configuration file.

I don't know exactly what this config.pro option does or why it should even be there...

file_open_default_folder working_directory <= what I have in mine

This may have something to do with how it behaves:

file_open_default_folder

working_directory, in_session, my_documents, pro_library, workspace, commonspace

Sets default directory from which to open a file when using File > Open.

working_directory—Searches the working directory.

in_session—Searches objects in session.

my_documents—Searches the My Documents folder.

pro_library—Searches the Pro/Library directory in Pro/LIBRARY.

workspace—Searches the Workspace in PDM application.

commonspace—Searches the Commonspace in Pro/INTRALINK.

default—Searches for the My Documents folder on Windows or for the working directory on UNIX. Subsequently, when you click File > Open, Pro/ENGINEER opens the directory where the previous File Open dialog box was closed. In a linked session with a PDM application, searches the active workspace. (link)

Hello Ganesh, I don't believe Backup has changed. As long as I can remember the backup function copies the assembly from your session with all its components to the directory you specify. If there is already a model with same name existing, it uses a higher version number. You are not closing the window before erasing in step #3 (i.e. your model is still in memory), right? If you do not clear your model from session (because it is displayed), it will be reused in the assembly. And if you do backup to working directory then, it should copy all components from session (i.e. your version of the model). Make a test by explicitly erasing everything from session and then open only the component model from your working dir. Gunter

Thanks Antonius and Gunter.

Gunter, I closed all windows and cleared the memory before taking the backup. If you put all your new models "In session" and open the assembly, everything works fine. The problem is I will be handling big assemblies and can't open and keep all new models in session since i do not know which sublevel parts ae coming inside.

I made a test with ProE and Creo creating some test assemblies and Creo behaves differently. ProE works as i expected.

Thanks.

This has to do with how Proe finds parts in an assy that you open. When you open an assembly, Proe will look for the parts it contains in the following order:

  1. In session.
  2. In the folder the assembly came from, regardless of if this is your working directory or not.
  3. Your working directory.
  4. Your search paths, if defined.

There are also Windchill paths in the mix somewhere, but I'm not sure where they fit.

So, if you want your modified parts to be inserted in that assy, you need to open them first.

This has been the order Proe uses for some time, going back I believe to WF1. Before that I think items #2 & #3 were reversed and I seem to recall there being a config option to restore the old order. I searched for it, but couldn't find it (It's not file_open_default_folder, that only sets the default folder displayed when selecting file > open. It has nothing to do with the order parts are retrieved.)

Is it possible that option was set in your install of Proe? You didn't say what versions of Proe & Creo you're testing.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

I never knew about 2), Doug. This is interesting.

I found a Google Books result that shows the order reversed as of WF1, so it looks like it was changed perhaps in WF2 or WF3. I'm currently working in WF4 and know the list above is correct there, by default anyway.

There was a time where Proe wouldn't find the part if it wasn't in your working directory or search path, but that was many revs ago.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

We recently upgraded to Creo 2.0 from ProE WF4.0. I tested using these two versions. If we can swap #2 and #3 of Doug's points, my problem would be solved. I have requested help from the support team of my organizaton. I will let them know about this conversation. Lets see...

I found an old internal PTC document about the change, which named the option Doug remembered. Ganesh, you may want to test with the hidden config.pro option "use_2001_search_order yes" (it still exists in Creo 2.0). But keep in mind that you have changed the default order, in case you get unexpected retrieval results at some point. After all the change to the order had been done intentionally, to avoid situations where you retrieve an assembly that has all components stored and end up with some components being loaded from the current directory instead. With this in place, when modifying and saving the assembly, some changes may be saved to a different directory than expected (the one that was current when retrieving). With the new method you can still replace components with those from current directory by opening them into session first, but it cannot happen unknowingly anymore. Gunter

dgschaefer
21-Topaz II
(To:gkoch)

Gunter,

That's the option I remember. In fact, if you Google use_2001_search_order, the first result is an eng-tips.com post where I replied. 😛

In my reply I linked to this PTC KB article on it, which explains things rather well.

--
Doug Schaefer | Experienced Mechanical Design Engineer
LinkedIn

"use_2001_search_order" has worked. With this option, Creo takes sublevel parts from my current working directory when I open assembly from other location which I wanted. Thanks Gunter, Doug and Antonius for your help.

This was a very enlightening discussion. Thank you for bringing it up, Ganesh.

Now I know I wasn't just paranoid... they really were out to get me

There is another wrinkle that caused us some confusion a while back. If you use the new failure resolve mode and use the "retrieve missing component" command, then Creo will remember the missing component's folder and add it to the search path - for the current session only.