dimensions not showing

[nrollins]

Hello everyone.



I am opening many drawings that I did the other day and I am seeing that
none of the dimensions are showing at all and the parameters are being shown
as ***. I seem to be getting chamfer dimensions and hole call-outs and
created notes (not dims.) This feels like the drawing is missing the model -
except, the drawing views are showing correctly.



I have PDF's of these drawings that have the dims shown. And yes I am sure I
saved them - there are ~15 drawings, I may have forgotten to save one or
two, but my memory isn't that bad yet.



Has anyone seen this and can give me any hints?



I am on WF5 with no PDM.



Thanks a lot!



-Nate


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[sl2741]

Hi Nathan,

*** indicates that your created dimension can not find the geometry (edges) that were used to create it. This is one of the reasons for using "show dimensions" that are created in the sketch of the model as they do not loose their association in the drawing.

My guess is that your drawings are not showing the "correct" version (dot number extention) of the model. So even though the geometry looks correct, the actual edges used to create drawing dimensions are not. This can happen when you inadvertantly create a drawing using a model from a different directory - for example after using "back up". So the model in session while creating the drawing is being saved to a different directory.

The "solution" to this particular problem is to locate the correct model (probably in a subdirectory or other directory) and open it into session. Now when you open the drawing, it will look at the model in session and if it is the correct model, the dimesions should appear correctly again. Now use file/back up on the part to get it into the directory with the drawing (or the directory that your drawing is looking). Exit pro/e or use file/erase in session to verify that you have corrected the problem.

Some users don't like to use show dimesions because they find it more difficult and slower, but I have been doing this forever and it does not take longer once you are use to the process. Ultimately it leads to fewer mistakes while creating the drawing. Of course there are times when creating dimensions in the drawing are the way to go.

Best of luck

Scott

[nrollins]

Well,



You guys are awesome - I am not sure what I would do without this community.



I received several responses; basically they boil down to three potential
and relevant issues:



1. Config option called: create_drawing_dims_only which sets where
created dimension info is kept (drw or prt)

2. File version is not correct (inadvertent deletion or saving prt
into wrong folder.etc.)

3. Can't think of a good #3, so I'm just going to type some crap to
make my list look longer so I look really smart.



While, I have certainly experienced and suffered from #3, in this case, my
troubles were in line with #2. Some idiot had the part files in a different
working folder. I still can't imagine how I did that.



#1 was enlightening to me - I can imagine that if the option were set to
"yes" (not default), then the info would be saved in the drawing and I would
not have noticed the issue until. who knows - possibly ending in a much
bigger mess.



Good stuff to know. Thanks again folks.



Happy Monday.



-Nate