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BenLoosli23-Emerald III
23-Emerald III
May 11, 2017
Solved

File marked as used when it isn't

  • May 11, 2017
  • 9 replies
  • 4258 views

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

Best answer by dschenken

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.

9 replies

M
mender12-Amethyst
12-Amethyst
May 11, 2017

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.

B
BenLoosli23-Emerald IIIAuthor
23-Emerald III
May 11, 2017

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
StephenW23-Emerald III
23-Emerald III
May 11, 2017

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.

T
TomU23-Emerald IV
23-Emerald IV
May 11, 2017

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.

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