File marked as used when it isn't

[BenLoosli]

We have created an assembly and added Comp_a to that assembly. We then decided to replace Comp_a with Comp_c, same type of hardware, shoulder bolt, but a modeled one instead of an imported one. The assembly has only been saved to the workspace and uploaded, never checked in.

Now we are trying to check in the assembly and Comp_a wants to be checked in, too, even though it is not referenced by the assembly. However, when we try to delete Comp_a from the workspace, it says it cannot be removed unless the assembly is removed, also. The Check in screen is also showing Comp_a as needing to be checked in.

Anyone have any hints as to what is hanging up the file?

My next step is to have the user remove all checked in files from his workspace, and then back-up the drawing and assembly to disk and then delete the workspace. Hopefuully creating a new workspace and pulling the file back in will solve it, unless there is a better approach.

Creo 2 m220

Windchill/PDMLink 10.0 m040

[mender]

I would venture a guess that you didn't delete the old component and assemble the new, but used some manner of Replace operation.  There are a couple flavors of replace, and I think at least one keeps a reference to the part, because the operation is reversible.  If that's it, I think there is the ability to say 'Break Dependency'.

Without seeing it, it's hard to be sure it is that and not something else.  If you have an SPR filed, it should be easy/quick for me to take a look.

[BenLoosli]

I will have the designer look into that in the morning. No SPR filed.

Unfortunately none of our parts can be uploaded for others to look at due to the nature of our business. Even Windchill log files must be printed and scan to be sent as PDFs, not text files.

[StephenW]

I remember those days!!

I know when I have used the replace command, there is often leftover data, even tho I have the "remember" option checked off by default AND sometimes it's drawing related, I think it might be attached leaders or created dimensions.  When nothing else work, I've used the cleanup dependencies option. Seems to help sometimes.

[mender]

We can do NDAs for keeping the data safe, though securing permission from your company policy might still be tough/infeasible.  For issues like this, you may be able to strip it down -- copy the assembly (including both the old+new parts) to a directory, then delete all features past the csys+datums from each, see that it still reproduces, remove all the other components from the assembly, see that it reproduces, then send the SPR with a no-actual-customer-data empty assembly with empty part with the question 'why does it reference this,and how can I make it stop?'

Conversely, if stripping out supposedly-unrelated data removes the dependency, you could remove the data more slowly and see which step does it, and narrow down to what is making the reference.

Just some thoughts.  Hope something works!

[BenLoosli]

Matt,

NDA's do not even come close to allowing my data out of my system. Classified DOE work. PTC hates it when I really have a problem and do open a help ticket because their first words on the phone are "Can we do a WebEx?" My reply is simple, "Not possible!" Then silence as the PTC rep tries to think what to do next.

I do have Creo running on an unclassified system that if I really need to show something to PTC, I can construct a pseudo model/assembly to imitate what is happening on my production system. This works sometimes, depending on what the issue is. In this case, The hints given may allow me to work through the issues with the designer in the morning.

ben

[dschenken · Accepted solution]

The default is to remember the replacement. To fix it use the reference viewer and look for the tiny trashcans. Those are references that can be deleted.

If you clean out the workspace and bring it from a back-up I think you will get ghost references because the replaced parts won't be in the workspace.

[dgschaefer]

dschenken wrote:

The default is to remember the replacement.

The config option "remember_replaced_components no" will default it to unchecked.

I added this to our config.sup as soon as I learned of the dependencies that remembering replacements would create.  Never could figure out why yes was the default.

[rmix]

I added this to my config.pro, and told my coworkers. This has always been an annoyance. Thanks!

[TomU]

Has everything been uploaded again since the component swap?  Usually uploading will make the server side workspace recognize the component is no longer required and the check in to proceed normally.  If that doesn't work then take a look at reference viewer in Creo.  It will show if Creo still see references between the model and the assembly.