Dimensioning Drafts

[mlocascio]

Pete Bokma,



Thank you for the suggestion. I think that what you are referring to would be A) A FAKE dimension on a drawing (if I went that way) or B) additional geometry in the model.



Please keep in mind that this draft is outbound. That may have some bearing on how it displays. Still, I would like to see a better way to display a draft dimension.



Michael P. Locascio



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[mlocascio]

This is an option – IF I want to create dimensions. Creating dimensions is what I do – IF I cannot find any better way.



Thanks

[DonSenchuk]

I just did a draft on a simple part and made a drawing. I couldn’t get it to show like yours.

[cid:image003.png@01CFBC7B.755EA550]

[mlocascio]

Donald,



Is the dimension on the left an added dimension, or is it a shown dimension?



Mike L.

[DonSenchuk]

Dimensions are all shown on that view.

[mlocascio]

IN-ter-rest-STINK…..



Is there something that I am doing wrong in the feature creation? There is probably a way to show a curve as a hinge, rather than a plane.



Mike L.

[DonSenchuk]

Let’s not call it “wrong”. Just different.

I’m not sure what that last bit means “show a curve as a hinge rather than a plane”. I used the edge as the hinge, nothing fancy. Or were you just thinking/typing out loud?

I’m curious if it depends upon how complex the face you’re adding the draft to is as well.

[DonSenchuk]

I created a new draft around all four sides as one feature, adding material to the base part.
[cid:image004.png@01CFBC7E.12E03B20]

[mlocascio]

Donald,



I think that we may be hitting on something rather important here. Can the hinge and the pull direction references be 2 different planes?



Mike L.

[mlocascio]

Donald,



I selected all 4 faces around the top (or bottom) surface to draft. Then I selected the top (or bottom) surface as both hinge and pull direction.



Mike L.

[DonSenchuk]

[cid:image005.png@01CFBC7E.E15355F0]

[dgschaefer]

Absolutely, and it’s incredibly valuable. The hinge controls where the surface will “pivot” and the direction controls where the angle will be measured from.

I’ve created draft features where the pull direction was 89 degrees off of the hinge.

--

[mlocascio]

Doug S.,



This is very good to know. I am not new to Pro/E, but sometimes these little nuances (nuisances) make all of the difference when we are designing.



Thanks,



Mike L.

[mlocascio]

Donald,



Thanks for your assistance. I hope that I helped some other folks see draft dimension creation in a different light. This is very good to know (and remember).



Mike L.

[DonSenchuk]

Anytime. That’s what makes this user list so valuable.

I’ve attached a small PRT file that contains all the examples I’ve shown for any users following this thread.

Edge hinge that adds material
Edge hinge that removes material
Hinge and Pull top surface
Hinge top surface, Pull bottom surface

While I don’t think I’m some kind of draft guru, let me know if I can help in any other way.

Don

[nrollins]

Agreed – thanks for enlightening me. I have notice the behavior but never took the time to understand it.

[mlocascio]

Now I want the group to repeat after me – No fake dimensions….. 🙂 (I had to get that in)

[mpeterson]

SentfrommyLGOptimusGPro™,anAT&T4GLTEsmartphone

[mlocascio]

There seems to be something missing in this message.

[rreifsnyder]

Please stop calling dimensions that are added in the drawing “fake”. They are absolutely valid dimensions unless you override the value. It’s hard enough to get people to open their minds to accepting another viewpoint without having them labelled fake. Both driven and drafted dimensions (saved with the part or saved with the drawing) will update if the features are moved/resized. The only thing they can’t do is to drive the model from the drawing, which IMHO is not a bad thing.

Rob Reifsnyder
Mechanical Design Engineer/ Producibility Engineer / Components Engineer / Pro/E SME / Pro/E Librarian
[LM_Logo_Tag_RGB_NoR_r06]

[mlocascio]

Robert,



I suppose that those fake dimensions are “valid” in terms of documentation. I strongly believe in the parametric system. That means being able to work both ways. When you add a dimension, instead of showing it, there is no way to make a simple change without interrogating the model. That’s just not productive, is it?



Michael P. Locascio

[nuheht]

I have had problems so many times with "fake" (aka created) dimensions. Created dimensions should only be used if there is no way if showing the dimension, as in complex surfaces. If the dimensioning scheme needs changed, I always change the model to reflect that and show the new dimensions on the drawing. Only takes a few seconds to do that and the end result is a much more robust drawing/model that you can pick the dim on the drawing to modify the model. To me, it just seems as the way to go, and I have been doing it this way since release 9. 



>

[BrianTaylor]

More salt to add to the wounds.... you can't fake it when you have a
requirement that your models are MODEL BASED DEFINITION. I.E. NO DRAWINGS
all information must be in the model and setup with annotation states.


Brian L. Taylor
Principal Technical Support Engineer
Hardware Engineering Center
Space and Airborne Systems
Raytheon Company
972-344-7697 (office)
-

13510 North Central Expressway
Dallas Tx 75243 USA
www.raytheon.com

Follow Raytheon On




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[ShandRonnie]

I 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.

Regards,
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

[mlocascio]

Model Based Definition is definitely a way to eliminate the added dimensions on a drawing.

[cdown]

I've always said added dimensions are a big no no!
That is why you buy a parametric modelling system.
I have worked in many companies and added dimensions have caused no end of
costly trouble!! If your model is created correctly then your design intent
is there thus no need for added dimensions.
I might be wrong but why dimension something twice & not know what is on
the drawing is actually what the model is??

[mlocascio]

Yes, of course it is faster and easier to create dimensions. But it is also extra work if the dimensions were already modeled in.



Fake is fake. When a dimension doesn’t come from the model, it is fake. It’s another AutoCAD drawing. If you want to do AutoCAD, they have a program for that.



Michael P. Locascio

[mlocascio]

Colin,



AMEN BROTHER!



Created dimensions should only be used as a last option. There are times when the only way to show the design intent of a feature is to create a dimension.

[davehaigh]

I see this has now devolved into the religious war over shown and created dimension.

Here’s my take on this.

There are many times where the design intent does not match what’s required on a drawing. Redefining the part just so you can get the dimension you want on the drawing can ruin the built in design intent of how it was modeled.

I’ve received parts that have almost no dimensions, because the engineer referenced features of the mating parts in the assembly. In that case, I’m not going to redefine his part just so I can show some dimensions.

In another case, we had a sub-assy that needed to show the range of motion. The skeleton drove the placement of the parts, but we needed to make weldment drawings that didn’t match the assembly structure. If we had tried to make assemblies that matched the drawings we needed the motion component of the design would not have worked. We made simplified reps and family tables to create the various weldment drawings.

There is no hard and fast rule. You do what you need to do to get the stuff out the door.

I use shown dimensions when I can, but I have no problem using created dimensions either. There’s no need to put Galileo on trial again over where the center of the universe is.

David Haigh
Phone: 925-424-3931
Fax: 925-423-7496
Lawrence Livermore National Lab
7000 East Ave, L-362
Livermore, CA 94550

________________________________

[jmoody-2]

I do see a distinction between created dimensions in part annotation vs. on the drawing. In the former case the ‘fake’ dimension lives with the part/assy i.e., if the drawing file is blown away the created dimension can still be shown on a new drawing.





John