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Family table instance not available for assembly

SOLVED
Regular Member

Family table instance not available for assembly

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

1 ACCEPTED SOLUTION

Accepted Solutions

Re: Family table instance not available for assembly

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

16 REPLIES 16

Re: Family table instance not available for assembly

Hi,

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


Martin Hanák

Re: Family table instance not available for assembly

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 Smiley Wink

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

 

Thanks again

Greetings

Vince

Highlighted

Re: Family table instance not available for assembly

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.


Martin Hanák

Re: Family table instance not available for assembly

Hello Martin,

thank you again. I've had a look at the trail file. Here is what happens (this is about a DIN913 part which has the same issue as the DIN7991):

 

! 9-Nov-18 07:24:03  Start C:\working_directory\d913_m4x3<din913>.prt.1
! 9-Nov-18 07:24:03  Start C:\working_directory\din913.prt.1
! 9-Nov-18 07:24:03  End   C:\working_directory\din913.prt.1
! 9-Nov-18 07:24:03  End   C:\working_directory\d913_m4x3<din913>.prt.1
! 9-Nov-18 07:24:03  Start C:\working_directory\d913_m4x3<din913>.prt.1
!%CEKann Variante d913_m4x3 nicht neu erzeugen.
! 9-Nov-18 07:24:03  End   C:\working_directory\d913_m4x3<din913>.prt.1
!%CE'C:\working_directory\d913_m4x3<din913>.prt.1' kann nicht abgerufen werden.
!%CEModell D913_M4X3<DIN913> kann nicht abgerufen werden.
!%CEKann Variante d913_m4x3 nicht neu erzeugen.
!%CE'C:\working_directory\d913_m4x3<din913>.prt.1' kann nicht abgerufen werden.
!%CEModell D913_M4X3<DIN913> kann nicht abgerufen werden.

 

Creo loads a generic file with version number 1 (din913.prt.1) from the working directory and complains that the m4x3 type cannot ("kann nicht") be created ("erzeugen") or retrieved ("abgerufen").

The version numbers of the generic part in my library are .6 and .7 (which is the one where I added the m4x3 type). Creo seems to get something wrong here. As I figure, the .1 number was created when the generic was first saved in the working directory at the first use of a DIN913 part which occurred a long time ago and Creo now fails to save the updated version, which would be a bug.

 

Greetings

Vince

Re: Family table instance not available for assembly

Hi,

1.] launch Creo

2.] open C:\working_directory\din913.prt.1 generic

3.] open Family Table dialog box

4.] select d913_m4x3 instance and click Open button

5.] verify all instances

 

 


Martin Hanák

Re: Family table instance not available for assembly

Note: If you upload din913.prt.1 I can check its validity.


Martin Hanák

Re: Family table instance not available for assembly

Hello Martin,

I did as you told me. The m4x3 type is not part of the family table of the generic din913.prt.1 file in my working directory. I solved the problem by deleting said generic from my working directory and pasting a copy of the din913.prt.7 file in my library directory and then re-retrieving the missing m3x4 parts from the family table of the updated generic. As I said, I now suppose it's a general problem. Maybe you (or anybody) wants to verify it:

1) Create a new assembly and insert a standard part from your library.

2) Save and close the assembly

3) Remove all parts from session

4) Now open the generic part of said standard part and add a new instance to its family table

5) Save

6) Reopen the assembly and insert a piece of the newly created instance.

7) Save and close Creo.

8) Reopen Creo, set the same working directory as before and reopen the assembly.

9) Creo should report the newly created version as missing because it (erroneously) did not add the updated version of the generic part to the working directory.

 

Can you confirm this is what happens? If yes, I think it's a flaw in the program.

Thanks a lot for your advice, I'd probably never have found the soultion without you. Keep it up mate^^.

 

Greetings

Vince

 

Re: Family table instance not available for assembly

Unfortunately I can't seem to upload the file because PTC's own forum can't deal with the version numbers of Creo files^^.

Re: Family table instance not available for assembly

Hi,

create zip file containing Creo file and upload it.


Martin Hanák