Won’t put radius dimension on entity

[Brett Bellmore]

I've been running into this problem lately, it comes and goes: I'll get a radius on a revolved part, put on as a round, or in the original sketch, and no matter how close I zoom in before picking on it in the drawing, it always selects one END of the radius, and thus I can't put a radius dimension on it.


For what it's worth, this doesn't appear to happen if I'm dimensioning a cross section rather than a regular view. Probably why I never noticed it before, I'm usually using cross sections to show internal features of my revolved parts, and just hit a run of parts without internal features.


Any idea what's going on?

 

[Knut Fiskergård]

Is it possible that the viewing plane makes the shape elliptcal?

 

[Brett Bellmore]

I considered that, but I always put my axis of revolution on the intersection of the front and right planes, and then use the right plane to cut my section. Besides, some radii will dimension, and some won't, in the very same view.


Ok, I just made a simple cylinder, by revolving a rectangle about one edge, and then put rounds on both ends. I then made a drawing with a general view of one end, and a projected side view. I can dimension the radius on one end in the projected view, but not the other end.


I converted the projected view to a section through the sketchplane, and now I can dimension both radii. Convert it back into a regular view, and the one end won't dimension again.


This is a bit freaky. But at least I can work around it by dimensioning only sections.

 

[dr_gallup]

Why don't you show the model dimension?

 

[Brett Bellmore]

Because it's a real pain compared to just dimensioning the drawing? And I shouldn't have to, the software should work the way it's supposed to?


But that does seem to function as a work-around, if I make a point of making each radius a separate round. Better than using normal leader notes, anyway. Thanks.

 

[jeff4136]

I wonder if it's a version specific bug, graphics card / driver / setup options
related, a combination of factors, etc? I just tried to reproduce the behavior
with the cylinder and rounds. If I zoomed out enough the end vertex is selected
and a "This dimension type not allow." error message generated. Zoomed in just
enough to make the arc silhoette easily 'pickable'; there was no probem.

 

[Brett Bellmore]

That could be it, based on searching this site, it's clearly not a common bug.

 

[airion]

Showing the model dimensions isn't nearly as painful as you think. I'd suggest you start using it because it is way faster to detail a part that way, especially when you create all your features properly with this in mind.


If you're annoyed that way too many dimensions pop up and you have to erase what you don't want, I have a suggestion for you. Just use the Show/Erase dialog box, show by Feature and View, then Select to Keep. Only the dimensions you choose will be shown.

 

[Brett Bellmore]

I have good reasons for dimensioning many of my sketchs differently than I dimension the parts in the drawing, (I've got features which fail when I change the part if they're dimensioned in the same way as needed in the drawing.) so dimensioning in the drawing is unavoidable. Given that, it's scarcely surprising that I don't want to mix dimension types.

 

[Knut Fiskergård]

I agree with Brett!!


I too want to dimension my sketches differently than how I want my drawings to be dimensioned. And I have many parts that don't have any dimensions because they are entirely created with references to skeleton parts.But the drawing part of ProE is not what it should (or could)be. I find it very cumbersome at times.


Another way to reduce the numer of dimensions from the model shown, when trying to find the right one, is to right click on the desired feature (or part) in the feature tree (in drawing mode) and select "show dimensions" or "show dimensions by view"

 

[Dell_Boy]

I often want to show dimensions that are not the original driving dimensions so I put in additional reference dimensions directly in the sketch. That way they stay with the part and you get the option of putting in extra section entities to make referencing to things like intersections and tangencies very close to arc end points easier.

However I still think that creating part dimensions in a drawing is a fail.


DB