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Ramax1-Visitor
1-Visitor
November 5, 2018
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Family table instance not available for assembly

  • November 5, 2018
  • 1 reply
  • 7499 views

Hi guys,

this is my first post so i hope I did everything right. Good old Creo is driving me nuts again: I have a legacy assembly for which i need a specific instance of a bolt (DIN7991_M3X6). Bolts according to DIN7991 are available in our standard parts library, but my needed size is not. No problem so far, I just created a new instance M3X6 in the family table and added this instance to my assembly. When opening Creo the next day, the M3X6 bolt is marked as missing. When clicking "assemble" and choosing the DIN7991 bolt, the M3X6 type is not included in the table that shows up.

And here comes the magic: When creating a new assembly or opening the DIN7991 part, the instance is available and can be picked without any problems.

I've spent some hours trying to figure out what the hell is wrong but can't find anything.

Can someone help me out on this one?

 

Greetings

Best answer by Ramax

Hello again,

indeed I'm using the academic version. It is true my understanding of Creo may not yet be as profound as yours but I'm working on it (which is the reason I asked the question in the first place).

My previous post was not entirely correct (the described workflow indeed works fine) but I think I got it now:

The problem occurred because the assembly I'm working on had been saved as a backup before I took over, which is the reason Creo saved the standard parts used at the time in the working directory and cut the links to the library. I first created the new instance in the family table of the library part, then opened my assembly (generic library part still in memory) and added the newly created instance to the library. Upon saving, Creo does not save the generic part that is now in memory but sticks to the one already present in the working directory (I tried the previously described workflow with a backuped mock assembly and could now reproduce the error).

 

Greetings

Vince

1 reply

M
MartinHanak24-Ruby III
24-Ruby III
November 7, 2018

Hi,

it looks like legacy assembly load old version of DIN7991 part. Look into trail file to check this idea.

R
Ramax1-VisitorAuthor
1-Visitor
November 7, 2018

Hello Martin,

thanks for your response. Indeed there are other DIN7991 bolts in the assembly. So what you are saying is that Creo will always retrieve the version of the generic part (and thus also the family table) that existed (and was saved with the assembly) when the first instance of the part was used?

That is interesting because it seems Creo is able to save the modified assembly (no error shows up) but unable to load it again. Does the program not realize that the generic DIN7991 part has been modified and the new version must be saved with the assembly? Looks like a(nother) bug to me 😉

You mean I should open the trail file with a text editor? What should I look for?

 

Thanks again

Greetings

Vince

M
MartinHanak24-Ruby III
24-Ruby III
November 7, 2018

Hi,

1.]

DIN7991 model can be located (theoretically) in several directories. Creo will load the first one he finds.

2.]

Start Creo, open assembly, end Creo. Then open trail file in Notepad. You will see full path to DIN7991 model loaded during assembly opening.

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