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Guys.. Please help !!

S

saravanans_87

New member
Guys..


Right now i have finished one drawing for a part. Then after that the part was modified by some one . Today when i update and see the drawing all the dimensions in my drawing is gone..


What happened??.. what went wrong??... Very Wierd !!(and am not very new to Proe and Pdm windchill)..


Now, what i figured is.. i can see those dimensions through the preview window, but not when i opened the drawing..


Any ideas... Please... share with me..


Regards


Saravana
 
Kenppy... No all my layers are in ON.


Am facing some many problems today...


1) some of my drawings i did previously, i can see the dimensions. But if some one else opened they can see only snap lines put by me.. & not the dimensions. (but they can view the dimensions in the preview window)


2) is it really necessary checking out the part or assy while doing updation in drawing?.. because.. if i check out the partor assembly along with drawing.. then save it and cheking it back again.. others can see all the dimensions..


Whats going on !!


Any help would be much appreciated.


Regards


Saravana.
 
what Pro/E version are you using?
If you have such possibility try to open the drawing in older/newer version of Pro/E.

I faced such(or at least similar) a problem sometime ago after a switch to FW4.0 from WF2.0.

It ended that I asked collegues who could open it corrwectly to save it, and then everything started to work on. Strange - I know.
 
Jacek..


Creo parametric 1.0


Guys.. any ideas.. am really wanted to do some thing regarding this..


(Am feeling very much bad on Proe for the first time in my life..)
 
have you tried saving as dxf and reimporting -- not saying this is the way to do it, but if the dims are there then at least that tells you something.
 
Kenppy.. No luck now also..


No AutoCAD, not evenAutoCAD viewer.


smiley19.gif
 
Mean while i had a chat with PTC guy, he told me to checkout the part or assembly when ever we are going to checkout the drawing, which is solving my problem (now, some how !!??)


Does it really needed ?..


Guys.. what's ur thought?
 
By default Pro/E / Creo saves the dimensions created in
the drawing in the part or assy file not in the drawing
file. This is done to allow associativity between
created dimensions and model dims and parameters. In
other words, it lets you add part dims and parameters to
the drawing dims via &[parameter_name] or &d14.

So, if you're working on the drawing and someone else is
working on the model you're going to loose all your
created dims when you bring their updated part into your
drawing.

You can set the config option 'create_ drawing_dims_only'
to yes to force created dims to be saved in the drawing,
but you'll loose the ability to add model dims and
parameters to your created dims. It'll work, but they
won't update.
Edited by: dgs
 
so first you`re using some kind of PLM - suppose PDMLink or Intralink, right?

second - you can check out only drawing untill all you do are changes related to drawing entities. Every chanhe of parameters taken from models, dimensions, etc makes associated parts to be updates, thus checked out(this is how PDMLink works).

However, note! - in Creo apart of layers you do have additional area in model tree where you can independly control visibility of views, notes, dims and so forth, check that!
 
Yeah, PTC guy and DGS are right. Whenever you are going to modify drawing you need to check out the model also. As proe is the parametric tool, drawing and model are associated to each other. A single change in the drawing or model reflects in model or drawing respectively.


Hope, I answered your query!!!!!
 
Guys.. thanks.. Great info.

But i was using WF3 for 2years and WF5 for 2years.
I used to checkout the drawing alone for modifications
without touching the assembly.

So, some changes in the model will reflect in drawing as
failed dimension. thats fine.

But now(croe parametric 1.0) all my dimensions
disappeared instead of failing..
Can some one explain this why?.
 
Nothing changed in this regard that I'm aware of. In the
16+ years I've been using Pro/E, dimensions created in the drawing are stored in the model file.

Many releases ago (2000i maybe?) they gave us the config
option to have them stored in the drawing instead
(create_drawing_dims_only), but the default I believe is
still no.

Is it possible that you, or your company, made a config
change from yes to no? Or perhaps you lost your old
config file from WF3 & WF5 and this option was not added
back in in Creo 1?
 
Doug.. i was not aware of this config things.


Yeah possibly, my company might change the wf3 & 5 config in such a way.


Actually i dont know.. any how.. very healthy discussions and learnings.. thnks guys..
 
Sorry to ask again the same question. Even though i am convinced by the answers.


Only one thing i want to make myself clear is stated below.


In detail : As Doug told, my admin might change the config of WF5 to "yes" in create_drawing_dims_only. So at that time it was working.


But even at that time, if some one else changed the model. I will seesome failed dimensions. So obviously we know some things has happened in the model.


Ok. Now, in Creo why all the dimensions are dis-appearing instead of failing.


Becasue i can see all the notes and even snap lines in the drawings except dimensions.
 
Created dims will fail if the thing in the model that
they referenced goes away. If so, they turn purple and
you have to edit their attachment.

But if you have the drawing open and add some dimensions
and save it, they get saved in your model file (having
the drawing open means the model is open too). If a
coworker also has the model open and is making changes to
it, then their changes are saved in their model file and
your dimension are saved in yours. There's no way to
merge both sets of changes into one file.

So if you close Pro/E and then open their model and your
drawing, those dims won't just turn purple, they'll be
gone because they never existed in their model.

Does that clear it up?
 
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