ghost objects

[#1]

I am uploading into PDMLink. When I save into a workspace, I get ghost objects. How do I find source of ghost objects in pro engineer. I need to resolve them for the checkin.

[ptc-914963 · Accepted solution]

Ghost objects are a pain in the ass in Windchill, some make since others don’t and shouldn’t happen but they do and you just have to find a workaround like everything else in Windchill. I will explain what we have seen, how they were created, and how we resolved the problems they created. Receiving machined part files or assemblies containing machined parts from other companies that use Pro/Engineer. Basically if they used Inheritance Feature or something like that to create the machining, when the file is Backed Up it does not include the casting automatically. It will allow you to open the machining when you try to but give you a warning. Now save that to your Workspace and Walla you have a Ghost File! To fix this, either contact the customer and ask for the casting model, save it to your Workspace and you’re good to go. Unfortunately most customers are not that accommodating and will not take the time to go back and send you the casting. So, for these set to No Server and then create an empty part with the same name, set back to the Server, and save to Workspace. You should get a warning that the same object exists, override it and save anyways. This will change your Ghost Object into the part the machining was looking for and then you can check in. Bringing in files from outside of Windchill that were Backed up to a drive can cause a random Ghost File once in a while. We see it with formats more that anything else for some reason. Also switching back and forth between Workspaces will sometimes cause it. We have users exit Pro/E and then re-launch Pro before switching Workspaces, this has solved many headaches. Basically if you have a Ghost file the first thing I always do is put a check mark in front of it and select Add to Workspace. Then next page that comes up is your tell tale of what to do next. If the file truly exists then this page will show you what it found on the server and let you download/add to workspace over the Ghost file. It is not always this easy but often it is. If it does not exist, that is when we create the empty file with the same name. Yes, it fills up the vault but it has not caused us any issues so far and we have been on Windchill for 3 years. The most irritating case of Ghost Files getting created is when a user has an assembly that has been saved to their Workspace and I can’t remember but I think maybe even uploaded but not Check In. Then someone changes their mind and the assembly changes. The user has to delete a part out of the assembly and add in a different part. The part that they deleted is not going to ever be used so they remove it from their Workspace and move on. Now when they go to check in it fails and come to find out there is a Ghost File in the Workspace with the name of the part they deleted from the assembly and removed from the Workspace. If you were to do a search on this in Windchill it does not exist anywhere. If you go into the assembly and look through the model tree or BOM it does not exist. So what gives? I then take and back-up the assembly into a temporary folder out on the local hard drive and find that its not there either. So I open the assembly file in a text editor do a search for the file and it comes up as existing within the file. Age old problem with PTC, their files, they don’t totally clean up themselves. With this all being said, it appears that Windchill digs deep into the Assembly file and finds this one line within the file that shows this deleted file number/name and treats it as a part that it needs. Needless to say there is nothing that can be done since you can no longer edit these files. So the only workaround that I have found is to create a empty file with the same name or find the original file in the users cache and bring it back into the Workspace. Sometimes we end up renaming the file to something like remove_�file name� hoping that maybe in upcoming releases of Windchill we can actually get rid of these unnecessary files, I have a folder full of these. I know that was a mouthful but I hope it sheds some light on Ghost files. If none of this helps let me know and I will see if I can help. Craig Clough CAD Administrator

[#3]

Thank you for your help it will help me explain what to do to my coworkers

[Darrell]

WF3 PDMLink 9 M020 We often get ghost items related to drawings. We rarely get them in assemblies, but the assembly drawings sometimes get outdated references attached to them. The way I have been getting around this is once you get the drawing and ghost item in your workspace, select the details page for the ghost item. Sometimes to get the ghost item to even show up in the workspace is difficult. Usually exporting and importing the drawing then updating everything does it. From the actions menu of the ghost item select replace and either search, browse or key in a valid model that is actually used in the assembly drawing. Type must match, i.e. part=part and assy=assy. It trades the ghost item reference for a valid item reference and allows me to check the drawing in without creating a dummy model with the name used by the ghost item. This method has never caused me any problems.

[MayurAima]

Is there any solution or script by which we can delete these ghost Objects on regular basis.

[ptc-877071]

the above examples work for models. For drawings the following is an exerpt from PTC Solutions - TAN 137288: "method is setting config.pro hidden option cleanup_drawing_dependencies to yes, launching Pro/ENGINEER when connected to a PDMLink workspace, opening the "having ghost" drawing, the user will be presented with a dialog listing the potential ghosts and asked to confirm their removal." The speed of light is faster than the speed of sound... That is why some people appear bright until the speak.

[RussDavidson]

In WF4, we are seeing that it seems to remember the names of parts that were replaced. If you see ghosts in an assembly, try using the reference viewer on the assembly and see if a "dummy" dependency exists for that part with the explanation of the dependency being "replaced model" and just break that dependency and save the assembly.

[jasonb1]

In the WF4 Reference viewer you can see and delete missing dependecies for assemblies that are created sometimes during a replace or deleting a component. This will allow you to break the need for the ghost objects. If there is a missing dependency to a drawing you can set cleanup_drawing_dependencies to yes, then open up the drawing. You would be asked if you want to delete missing references. If you do this you will not need to create a dummy part to satisfy the ghost objects.

[Bucknut]

Jason

This may sound simpleton to you but where do I find this "cleanup_drawing_dependencies" prior to opening a drawing? Not a 'trained' WC admin.

MS

[JamesBurcham]

Its an option in the config.pro for Creo/Proe

[smilliman-2]

Is this still an option or did they change the name? I can not find it.

[LoriSood]

Scott,

It's still a valid config.pro option. However, it is hidden so it won't appear in the config.pro editor. You have to type it in.

[cspinelli]

Lori,

i set cleanup_drawing_dependencies to yes in config.pro but, when i open the drawing i have no request to clean up ghost.

we have Creo 2 M140 and Windchill Release: 10.2 M020-CPS05

[TomU]

You have to open the drawing from local disk, NOT from the workspace.

[cspinelli]

ok, and inside workspace is not possible?

[TomU]

Nope. The config option only applies to files opened directly from disk.

[TomU]

Generally I will open the drawing (from the workspace), do a file backup to the desktop, erase the drawing from memory, then open from the desktop.

[cgorni]

Root causes for Ghost objects may be different and usually require deeper analysis of the Data and relationship between objects, some expertise is needed.

You can refer to article CS20956 to get more details, illustration and solutions depending their nature.