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Created vs shown dims


Created vs shown dims

body{font-family: Geneva,Arial,Helvetica,sans-serif;font-size:9pt;background-color: #ffffff;color: black;}Ronnie,
While I agree that created dimensions have their place, I also feel they should be used sparingly, and some of your examples show why.
CORRECTLY placed created dims represent 100% size of the model. This is easy for a machined part, but if you have draft, or have features that are not orthogonal to the view, you can wind up with oddball dimensions that do not reflect the intended size and/or can be misinterpreted. This gets even worse when you are using surfacing where little is orthogonal to the view.
Companies where one person models and another does drafting is even more important to use shown dimensions, as you can quickly lose the design intent if the modeler viewed it one way and the drafter another.
Personally I use created either as a last resort, or when it would be too complex a change to go back and re-dimension a feature way back in the model tree. They do have their place and I do use them, just as little as possible.
41. EXTERNAL: Dimensioning Drafts (Ronnie Shand)From: Ronnie Shand
Subject: EXTERNAL: Dimensioning DraftsI totally agree here with Robert.

Here is the definition of a created dimension:
Created dimensions are in no way fake dimensions.
Created dimensions represent 100% the size of model.
Created dimensions are the true value that Pro/E computes from the model been shown in a drawing view.
If the value in the model changes, the created dimension will also change and update in the drawing

Many times it is faster to create the dimension than to show it by find it in the model.
Some companies have designers model all the parts and then a complete different department makes the drawings.

Ronnie A. Shand
Staff Mechanical Design Engineer
Lockheed Martin Mission Sensors & Training MST
100 East 17th Street
Riviera Beach, Florida 33404
Phone 561-471-4342

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Really replying more to Rob, but...

Created dimensions are candidates for being overridden, hence are the only ones that can be easily faked.

It is also easy to create references to geometry that look almost right, but are subtley wrong, such as selecting the end of a line segment, not noticing a small round.

Created dimensions can also carry unwanted results. I believe if a line has an end-to-end dimension created, and a round added, the dimension, which should be to the intersection of the line and the next face, will instead not include the length of the round. The value change is automatic, but the meaning change is wrong.

The ugliest problem I've run into was a casting/machining where a contract engineer was given a hand-drawn drawing with about 150 (or so) dimensions, and missed where the origin was. So he built the model entire model dimensioned from one side and created the 150 dimensions on the drawing. Bad news was: the intent of the redraw was to change the design slightly. In some cases, to change a wall thickness which was one dimension on the original drawing required going through a stack of a dozen dimensions to get the desired result.

What should have taken one minute to do instead required a full re-check of the model and the drawing to make sure nothing else was changed incorrectly in determining which dimensions affected the wall thickness and what the new values needed to be.

Usual disclaimer - tools used poorly produce poor results. It's just that created dimensions are more easily poorly used.


The ages-old debate, created vs. shown dimensions...

My two cents: if you had asked me a year and a half ago, I would have been squarely in the shown dimensions camp. I used to tell everyone that at least 95% of the dimensions that appear on a drawing should come from the model.

Now... I'm split. What caused the change? Flexible Modeling Extension and 3D Annotations. Incorporating Direct Modeling into Parametric Modeling is powerful, but requires us to rethink modeling conventions. With Model Based Definition, there are differences between the way that feature-owned and non-feature-owned dimensions behave, and I haven't figured out all the nuances and repercussions yet. As a result, I'm no longer firmly on one side or the other of the issue.

David R. Martin II

Senior CAD Application Specialist


The problem I have with shown dimensions is if I toggle them to ordinate in the drawing they convert to ordinate in the model. The ordinate dimensions then become difficult to work with in the model. Does anyone else have this issue?

I find it interesting this question rears its ugly head every so often. In the rush to get it all done at light speed, things tend to get overlooked.I will get the Old School CAD monkey stuff out of the way first. Drawings have been and still are an important and integralfacet to the product. In many cases the drawing is the contract between your company's supply chainand the supplier. In today's faster, faster, faster workplace, drawings seem to get dismissed and marginalized becasueof misused"CAD is Master" statements on drawings. Keep in mind, this process works best when every player in the product chain has access to the CAD and is capable of using it correctly. If one link in the production chain is incapable to read CAD or measure per the data, it is all for not.

Both created and shown dims have advantages and disadvantages. I use a combination of both becasue view orientationon drawings can work against you with placement of particular dims. Also, it is typical that as I model things I do not know exactly how I need to inspect a part so my "shown" dims do not present as I need them to. I may, if enough time permits, will redefine features to allow for shown dims. Other times, I do not have time to change the model. It's great to have the freedom to do both.

With that said, I emplore you all to sweat the details on your drawings no matter which "standards" your respective organizations use. What I mean by that is make sure your details are done well. Never assume the drawings "update" automatically. Whether you use created or shown dims has always been a matter of care and attention. In other words, good detailing skills are required regardless of the method used.

The same thing happens when you set tolerances to limits. The model dimension is reset to the midpoint of the limit. That's why we always use created dimensions when using limit tolerances.

David Lawrence
Sr. Mechanical Engineer
Sigma Space Inc

Isn't there a setting that allows a user to set the tolerance without it
affecting the model?

Michael P. Locascio

5-Regular Member

maintain_limit_tol_nominal (yes, no)

Maintains the nominal value of a dimension regardless of the changes that you make to the tolerance values.



Thank you Tracy Willis! I was pretty sure that there was an option for that.

Michael P. Locascio

Is there a similar option for plus-minus tolerances that I can turn off? For example, I want the geometry for dimension 100+0.04/-0.02 to automatically be at the middle size (100.02) instead of the nominal.

Janet Grove

This is precisely what I would like to avoid doing if I can. If I can’t, then I can’t. But I was hoping someone had a trick up their sleeve.

Kind regards,
Janet Grove

23-Emerald IV

I don't remember the name, but there is a command you can run that will automatically change all dimensions to be centered in the tolerance range. I believe this is intended to be used prior to export for other downstream suppliers. If I remember right, this centering change is lost the next time the model is regenerated. I'll see if I can find it...

Tom U.
23-Emerald IV

Found it. Dimension Bounds

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