cancel
Showing results for 
Search instead for 
Did you mean: 
cancel
Showing results for 
Search instead for 
Did you mean: 

Drawing Checkin; Unassociated Part is Being Checked in Too

wbottis
Amethyst

Drawing Checkin; Unassociated Part is Being Checked in Too

Hello,

Another obscure Creo issue that I will try and describe.  I just attempted checkin of a new drawing.  The assembly was checked in by itself already.  Upon checkin of the drawing, a new part having nothing to do with the drawing is being checked in.  This same part did not "want" to be checked in with the assembly, only the drawing.  Where is this link taking place and how do I break this link?  Thank you.

Tags (3)
8 REPLIES 8

Re: Drawing Checkin; Unassociated Part is Being Checked in Too

More than likely if you view the details page for the drawing and/or the part, you will see a reference from each to the other on the 'Related Objects' tab.

 

How the link was created is a whole different issue.  Things I normally check:

  • Has the part been added directly to the drawing?  (Look at the drawing's drawing models.)
  • Does the part have any references to the assembly?  (Check the assembly's reference viewer and both object's 'Related objects' tab in the embedded browser.)
  • Is there a relation reference to other parts anywhere?  (Something referencing this object's session ID?)

If the only link is between the part and the drawing, and there are no other links from this part to the assembly or any other parts, then usually I go down the path of backing the drawing up to disk, erasing it from session, removing it from the workspace, removing the offending parts, and then reopening it from disk with the config option "cleanup_drawing_dependencies" set to "YES_CS_NOT_REQUIRED".  This should pop up a box giving you the opportunity to permanently remove this (now missing) reference from the drawing.

Re: Drawing Checkin; Unassociated Part is Being Checked in Too

Is that part shown on the drawing?

I have attached a test part to a drawing template one time by mistake. Not shown on the drawing, but still loaded with the drawing only.

 

Re: Drawing Checkin; Unassociated Part is Being Checked in Too

no, the offending part was not added to the drawing independently, I have double-checked.  The only model associated with the drawing is the assembly.

IRe: Drawing Checkin; Unassociated Part is Being Checked in Too

If that part is in the assembly that is in the drawing, it will always check in with the drawing.

If you don't want that part to check in, undo the check out.


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Re: IRe: Drawing Checkin; Unassociated Part is Being Checked in Too

The offending part is not part of the assembly.  At one point it was.  Then it was replaced by copy.  The link remained in the drawing, but not the assembly.  I have a smart table (on-drawing PL) in the drawing.  Possibly the smart table is holding the old session ID as Tom U mentioned.  I had updated the smart table prior to checkin to preclude this.  Maybe that was not sufficient.  

Re: IRe: Drawing Checkin; Unassociated Part is Being Checked in Too

Please try the solution with the config option "cleanup_drawing_dependencies".  We have lot of problems with orphan references being left on drawings and I'm starting to think it's directly related to Creo's 'replace by copy' functionality.

 

Here is more info on that config option:

https://www.ptc.com/en/support/article/CS28858

 

Re: IRe: Drawing Checkin; Unassociated Part is Being Checked in Too

I haven't had to use the cleanup drawing dependencies option in a while but I have used it a lot in the past.

Make sure you follow the instructions in the support document link Tom posted. I always had to do it twice because I would do something wrong and don't forget to remove it after using it.


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Re: IRe: Drawing Checkin; Unassociated Part is Being Checked in Too

I don't necessarily follow all the rules and warnings in that article.  I leave the config option turned on for everyone, all the time.  (It's in our company config.)  Since we normally work from Windchill, it never comes into play unless someone intentionally backs up a drawing to disk, and then reopens it from disk (and there are missing objects.)

 

I've learned that most of the time you don't need to remove the offending drawing from the workspace, you just have to erase the one drawing from session, reopen it from disk, save it to the workspace (hit 'okay' to the conflict warnings), and then use the workspace 'update' command (with 'reuse' - the triangle icon) to 'snap' the 'new' workspace object back to the server copy.  From there you can just check it out and then check it back in.  🙂

Announcements