Updating dimensions

[alwaysdrunk]

Hi guys


I have one question. When proe modelsare modified, dimensions on its corresponding drawing becomes outdated (turn to somewhat violet color). Is there any way i n proe drawing to automaticaly update outdated dimensions with one regeneration click? because I am updating it manually, I have no Idea on how to do it quicker when there are dozens of dimensions. Thanks for the help if any.

 

[robertib]

Unfortunately, dimensions created soley on the drawing are not parametrically linked to the CAD model. Thus when changing the dimensions in the model, the drawing ones don't update.


Thecorrect

way todo thisis to use the Show/Erase to show the dimensions from the model - of course this only works when you can design the model with the dimensions you want to show, which is not always possible.


A workaround to get the correct dimensions to Show on the drawing is to use points & relations, but that is a complicated work-around.

 

[vlad1979]

Dimensions created in drawing are "parametric" and do update when you modify the part.


BUT they update only if they don't loose the references (say you modify the part length the created dimension in drawing will update).


Your dimensions are "magenta" in colour because you deleted or redefined a feature in part and the dimensions lost the references. Your only choice is to delete that dimension and create it again, or to right click on it edit attachment and choose the new attachment.

 

[alwaysdrunk]

thanks guys,


Got the same answers from my colleagues here.in short "There's no way". I'll just make some tweak-the-proe thing here. thanks anyway.

 

[dr_gallup]

Like robertib said, the CORRECT thing to do is use shown dimensions. Also, if you have to use created dims attach them to stable references like datums.

 

[cbenner]

The CORRECT thing doesn't always give you the DESIRED results. For instance, we use Pro Piping, and do not always have control over which dimensions are created as we route pipes. These dimensions may or may not be what our shop needs for fabrication. Sometimes dimensions HAVE to be created on the drawing.

 

[dgs]

There's some confusing information in here.


Dimensions created in the drawing definitely DO update with changes to the model. However, if the edge or vertex that dimension references goes away, the dimension will fail. Just like a feature fails of it's reference goes away. Some times this is unavoidable, but with careful reference control you can prevent some of this.


There's no universal right or wrong way to make your drawing dimensions. For many companies, shown dimensions are the preferred method. For us, created dims are preferred because our model dims frequently are not the dims we want to show on the drawing. Many times, there are no model dimsbecause the geometry came through a copy geom from a skeleton. Frequently, the desired drawing dimension scheme changes. With created dims, those changes can happen in the drawing instead of having to go back and find the dims in the model and redefine the feature. Lastly, if the model changes and a feature dim is deleted, it just disappears from the drawing with no evidence it was ever there. With Created dims, they remain, but turn purple.