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Newbie Question - Dimensioning drawing views


New member
Hoping someone will help me through this particular phase of my ignorance.

If I...

Create an extruded plate, say 5 x 5 x 1, set up a drawing view looking at a 5 x 5 face, then dimension it (driven dims, pick edge - place dimension).

Go back and chop off part of the plate with a cut. It's now 4 x 5.

Go back to the drawing and the dimensions are still 5 x 5 with a node hanging off in space. (I think I understand what's happening; the dimension is linked to the feature edge?).

Is there a way around this behavior, such that the drawing dimension will reflect the edge length projected to the drawing view without regard for the feature(s) the length is dependant upon?


Jeff Howard

yes, But you forgot the regeneration function. And ... what I don't understand is ... why you chop the plate when Pro/E have such powerful modify/redefine tools?

Anyway, If in your 2D drawing you will use show dim. you can modify the part from 2D to 3D.
Thanks for the thought and reply.

I had regenerated the model and drawing when I noticed the problem.

Where I first stumbled onto this was while working on an imported (via STEP) assembly that I was finishing and documenting (no driving dims to show, but they would act the same). I had created a prelim drawing set, after which I trimmed the piece in question to clear an added part. Going back thru the drawing set for the release version is when I noticed the anomoly and the plate example was done trying to figure out what was going on. I thought it might be due to the imported components and wanted to see if the same would happen with native parts. After seeing that it does happen with freshly created geometry I'm assuming it isn't an anomoly, but normal function (?). Even given that the original part wasn't imported geometry I'd have probably done a native part the same way if there were features referencing the edge that needed trimming.

In the end, I guess I just want to verify that what I'm seeing is normal for the conditions (Pro/E is completely new to me) and I can act accordingly. If there's a way around the behavior, even better.

Thanks, again.

It sounds like you've transitioned from a Boolean operator to Pro/Engineer, which is a feature-based modeler. It does require a change in the way in which you approach design.

In Pro E, you want to create and design your features with the dimensions and parameter that you want to control, those that reflect your design intent.

I would say the problem in this case isn't how you're documenting your drawing, it's how you're creating the model in the first place. Maybe instead of trimming the part so it clears the added part from the assembly, a better way to approach the design would either be to:

1. Use a data sharing feature like Copy Geom to bring the important geometry from the added part into the first part for designing your features so they are the correct size.

2. Consolidate all important geometry in a skeleton model, and use Copy Geoms to control the original model and the added part.

Yes, this requires more work up front, and adds complexity to your models, but your models will be more parametric and robust-- so when you need to make a design change, you make one change, and the other models will update automatically when you regen the assembly.

David Martin

Torgon Industries
Thanks for the reply, David.

Actually, I'm transitioning from Adesk Inventor which does support, and I am familiar with, the methods you mentioned.

What I was trying to get a handle on was the unexpected behavior of the dimension. I think the short answer is that the dimension is owned by a feature edge (or the sum of features at the time of placement) and not by a projected part (sum of all features) edge which is the behavior I'm accustomed to.

Have a good one,

Jeff Howard

Yes, technically the dimension is owned by the feature (not actually the edge or any other geometric entities); the dimensioning scheme is determined by the references you choose for locating your feature and the sketched entities that determine its shape and size. The dimensioning scheme is not determined by the Boolean result of your features and feature operations.

And a good rule of thumb is the overwhelming majority of the dimensions that appear on your drawing-- at least 95%-- should be feature dimensions that are shown, not created dimensions (assuming you're detailing a native model).

David Martin

Torgon Industries


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