Using Creo 4.0 (no Windchill)
I find that if I have the drawings open for (4) parts: A.drw, B.drw, C.drw, & D.drw and that these for parts are contained as instances in a family table of Generic - ABCD.prt, that when I verify the family table (and I get "Success" on all for instances A, B, C, & D) that when I go to any of the drawings, I need to regenerate the drawing to get rid of the little yellow dot.
If I just verified the family table, why is the model in the drawing wanting to be regenerated? I am not doing this in the proper order in order? Sometime I regenerate the instance and save the drawing is says that the other instances have not been regenerated.
Solved! Go to Solution.
I think I found the issue causing the regeneration issue.
I had a couple of relations in the part file:
/*creates MASS and VOLUME using MASS_PROP_1 feature
Two different solutions worked and I tested both.
-The first was to comment these two relations out by adding "/*" in front of both lines. After doing this, when I verified the family table (FT) the drawings stayed "green" dot status. If I changed the FT (without verifying) and went to the drawings, they were all "yellow" status. Go back to the model and verify the FT and they were all "green" again.
-The second was to move these relations from the "Initial" to "Post Regeneration" tab.
Then after verifying the FT, the drawings remained "green" dot.
Hope this helps someone else too.
Do you have post-regeneration relations in your FT generic?
The drawing may just be flagging that the FT has been regenerated and so the drawings needs to be also?
If you verify and save the FT, then open the drawings, do they show the yellow dot for regeneration?
What are post-regeneration relations?
I will check about the regen if the drawing has been opened after the family table (FT) regeneration.
When I added a dimension to the family table (didn't change the values of the dim, it just wasn't in the family table) and then verified the family table (all instances were Success"ful") and then opened up one of the drawings from the family table, the little yellow dot was there "begging" for regeneration.
I did a regeneration on the drawing, save it. Existed out of everything. Erase all. Reopened the generic and deleted the dimension that I just added. Verified the family table. Opened up the same drawing and "lo and behold" the little yellow dot reappeared.
Open the relation editor, in the lower right corner is a drop-down that says Initial. Click the arrow and you have the option for Post Regeneration relations. In family table parts the weight will not update unless it is done as a Post regeneration relation. I use this for all of our hardware items so we can get the weight into the assemblies.
A new twist tested.
I regenerate the drawing. Save the drawing. Erase all not displayed. Reopen the drawing and the little yellow dot is asking for a regeneration? Why? Nothing has changed other that I removed the model from the memory and it has to recall it.
Do like I do, ignore the little yellow light and all your problems go away!
Seriously, do you use Windchill PDMLink? I lock my files in PDMLink so they don't regenerate and that solves some of these issues.