Ghost parts

[JamesBurcham]

My company installed Windchill a couple of month ago and we have been seeing a lot of ghost part issues, with the items that we imported into Windchill. As a company we used Proe without Windchill or any other data management software for over a year, so we had thousands of models that we imported. The problem we are having is that when we try to revise or copy any of the assemblies we imported we are getting several ghost parts and cant find a way to resolve them so we can check in our work. We have tried using the Auto Resolve at check in, but that isnt working. The ghost parts that are being created are things that dont exist anywhere and no one seems to know what that are. My guess is they are old items that were at one point part of the assembly, but where removed some time before they were imported into Windchill. If anyone has any advice on how to resolve ghost parts it would be appreciated.

[BuddyHudson]

Hey James,

We have had many issues with ghost objects as well. I think some of it has to do with users modifying assemblies without pulling the drawings into session. The drawing is still looking for some models that don't exist in the system any longer. I agree the auto resolve just does not work (like it should). You can also use the Reference Viewer to look at the references and dependencies and see if it will allow you to "break dependency" to the missing dependent. Once you break it, save and refresh your workspace, the ghost should go away. This works sometimes, but sometimes the system will not allow you to break these. We have even come to the point that sometimes we just simply create a new part with the name it is looking for that is emtpy, so we can get all the other objects checked into the system.

Hope this helps,

Buddy

[JamesBurcham]

Where do I find the Reference Viewer, is that the same as the relationship explorer?

[JamesBurcham]

I found the reference viewer, I was thinking Windchill not remembering the reference viewer was in the actual model. For the one item I tested this worked and I was able to to check in.

[StephenW]

There are a couple of config.pro options (hidden options) that MIGHT help cleanup references.

cleanup_drawing_dependencies YES

cleanup_layout_dependencies YES

These sometimes will pop up a window saying the references can't be found and you can delete them.

I would advise you put these in, restart pro/e with them in and then open the assembly or drawing or part. See if the pop up window comes up. Delete the references, save. Remove the options before continuing since they may not be predictable.

These are hidden options so the search will not show them, you have to manually add them.

Good luck,

Steve

[JamesBurcham]

I added these and I didnt get a pop in my model. I have removed the dependencies, but I still have ghost parts that are preventing me from checking in my items.

[StephenW]

If it finds the "missing" dependents, it should open a window like below. If it doesn't, come up, then it probably isn't whatever kind of dependent it is looking for. For me, it finds them about 1/2 the time.

Just to be clear, you restarted CREO with these options already in the config, correct? These options can't be turned on or off in a session, you have to have in the config.pro before you launch that session.

Also, don't forget to remove these options after you have finished. The option is hidden because PTC doesn't support you if it messes something up.

[JamesBurcham]

I did restart Creo after turning the options on. I have opened about a dozen models and resolved ghost part issues, that box has not popped up once. I think our issue stems from importing our files into Windchill. I have been able to bread the dependencies so for now I'm just moving forward with that so we can keep working.

Thanks everyone for the help.

[LoriSood]

As an FYI... there is a bit more to the cleanup_*_* options than just closing and restarting Pro/E. You also have to backup the files to disk and then retrieve them into session from disk--not from the workspace. It's a bit convaluted, but it's what is required to make Creo look for the old dependencies.

CS28858 explains how to utilize these options.

Note: The Auto Resolve Incomplete Objects preference only works on dependencies that Windchill/Creo doesn't treat as required.

[StephenW]

Thanks Lori, I had forgotten about that. It has been a while since I had used it.

Steve

[JamesBurcham]

Thanks everyone for the help, I have learned more about ghost parts then I ever wanted too. Using the different things you all have said I have been able to resolve the current issues we have with the ghost parts. The only problem I'm still having is I have hundreds of assemblies that need to be fixed because of these ghost parts. If anyone is interested in doing this for me so I don't have too I would really appreciate it.