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Dimensioning Philosophy

I have stated (very tonge in cheek), that the create dimension functionality should be removed from Pro/E. That is of course a joke, there are many times when created dimensions are needed. And, when part level dimensions need to be "shown" in an assembly drawing absolutly required. (I have accidently changed a part by using a shown dim at the assy level and editing it for what was needed there.)


For part drawings, what I do is:


1.Create the views needed to show the part correctly.


2. Show dimensions on a feature by feature basis.


3. Review the drawing to add dims that are needed for the drawing, but not the model (i.e. dims to center a feature that is centered by design intent).


Do I think it is necessary to be able to change the part from the drawing, no but it is nice. What I do think is (when the drawing is king as it is for the most part now), showing dimensions is the best way I know to insure that the part is completly dimensioned.
 
I prefer to use Shown dimensions on my projects, whenever possible. I find it faster and easier for me to detail a drawing using shown dims (feature by feature). A drawing that doesn't use "shown" dims takes way longer to detail.


Being able to make modifications to the part from the drawing is just a bonus. If you are not sure what themods will affect, you probably shouldn't be doing it in the first place.


I was recently burned bybeing forced to use manually created dimensions; An engineer gave me a model to detail.When I picked on a line to dimension it, it grabbed another line near it that was "hidden?". When I open up the model to see what the offending feature was, I found all kinds of junk features that had no relation to the final part.They were hidden, suspended, cut out, etc. that were left over from his design process and the "part" that he used to duplicate from.
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If I had been using shown dims, it would have saved me the headache. Of course, almost none of the dimensions he uses to build a part, are usable in the drawing, due to his modeling methods.
 
This is one of those ancient strings that appears to have been resurrected when the server crashed. But it's a relevant one, and I'm not sure if I have put in my two cent's worth on this topic.


I have always used created dimensions exclusively on drawings, and lack of functionality in Pro/E is a huge minus. While many feature relationships (and dimensions) that make sense in the model (and the assemblies where it is related to other features in other parts), they are of little meaning to anyone fabricating the part, especially if a skeleton model or master model is used. So 'show dims' can generate little more than confusion for the fabricator. Also, some dimensions always need to be created: this makes it difficult to figure out which are created and which are simply shown, esp. if the user trying to edit the model/drawing didn't create it originally. Editing shown dimensions is a open invitiation to disaster in many cases: the model crashes, and the user has to dig into the model anyhow. Yes, having separate dimensions in the drawing and model does require some intellect on the part of the designer to produce a set of dimensions and datum references in both files that will reflect his design intent and still be producible and inspectable. But that has always been part of being a mechanical designer, whether CAD tools were used or paper drawings made by hand. The folksin PTC Sales push 'the magic space helmet' concept to the hapless management at their customers, touting the power of shown dimensions and the time that can be saved by using them. But shown dims just make for more work in altering either the models or the drawings to get something useable on both sides (design intent and manufacturable parts). It's better (and easier) just to keep the two worlds separate, and exercise your skill as a designer/engineer.
 
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Nice way to sum it up.


I can't remember the last time one of my models crashed. Since I started tying parts to the co-ordinate system, my assemblies have been rock solid also.


I don't understand how you figure that "shown dims just make for more work in altering either the models or the drawings". I'm not asking for an explaination. I just don't get it.
 
I have disabled changing dimensions in the drawing, to prevent accidental change of dimensions. When I want to change a dimensions I want to check in 3D anyway if it is correct.

Also for freeform surfaces (design geometry) is often is impossible to use (only) shown dimensions.

Most importantly: for the plastic parts I work on it is (nearly) impossible in many cases to have shown dimensions, because of the drafts (which often en in freeform surfaces) and the complexity of the features. Often you either can't create a functional region like e.g. a snap-fit hook, sometimes consisting of over 20 features in the tree, taking into account that in some specific area you want to place a shown dimension. Or when you theoretically can, it is too much work and unproductive. When it's possible to use a shown dimension, that's great, but dependent on your part it can be impossible or in some cases simply too much work.

A useful workaround to have a stable 'shown dimension' in some cases would be to create the dimension in the 3D part, using stable references and then showing that dimension. For example the maximum width of a freeform part can be determined by 2 analysis features each placing a datum point on the outermost point of the surface. Then I create a dimension in the 3D model between these points. Easy and stable, but it takes a bit more work and features.


Edited by: Zestje
 
It's very simple. Once you finish figuring out which view you want particular dimensions to appear in, figure out how the machinist will actually make the part and how the inspector will inspect it, the dimensions you used in the part sketches and features aren't particularly relevant. This is because you created the model in the context of the assembly. Of course, you can always simply show the model dimensions in any view, forcing the machinist and inspector to interpret what you are trying to create. This is likely to result in nothing but tears.


Every experienced designed and engineer I know uses created dimensions in drawings exclusively. Indeed, many companies specifically prohibit the use of shown dimensions in drawings. Those individuals I know of who advocate shown dimensions are of questionable competence or lack hands-on experience (management and PTC instructors).
 
Thats a bit arrogant Mindripper.


If I work for a company that insists on shown dimensions (and some do) I redefine the features (if necessary) to be able to display them correctly.


I also have no problem with created dimensions. Sometimes they are necessary if you need to override the default dimension with some other data, as you cannot use @o with shown dimensions.


Using shown dimensions can speed up drafting work if youcopy the same base part to makenumerous similar ones. Plus you will always know you have the same dimensioning scheme on each one.


Using shown dimensions forces you to contain all the dimensioning and tolerancing data in the model. Thisis useful if you want to send the model out for detailing, say, in another country so you can be sure they dimension it correctly by insisting on shown dimensions only.


Both methods are acceptable. The printed result should look the same, either way.
 
It makes no difference whether the drawing dimensions are shown or created: they are still tied to model features, and will vary with the model. Yeah, all of the same rules apply - plus a couple of bonuses with created dimensions: no need to redefine themodel to suit the printand no mixing of dimensioning schemes. I don't have a problem with shown dimensions either: I have used both, but find created dimensions to be much less work and far less of a headache, especially on complex parts or parts used in multi-level assemblies. And I'm not the only one: every experienced designer or engineer I have worked with using MCAD over the last 25 years is of the same opinion. BTW: this has proven to be true for users of a variety of MCAD systems, not just Pro/E.


I'm fundamentally opposed to the whole concept of sending out models to be turned into detailed drawings by someone other than the person who designed them. No one understands the design intent like the designer, and many design errors/improvements are caught during the drawing creation phase. Yeah, I hate detailing drawings, but nobody knows my parts like I know them.
 
Oh the luxuries some of you have.

95% of my parts would not be possible to do exclusively shown.

I have been in the auto industry for 15+ years and for the past 7 of them, my parts start as a stp or iges file from a customer. most of these parts come from crap surface files from the OEMs. I feel extremely lucky when I get a base part that even solidifies on it's own. Most of the time I find myself in the import data doctor trying to get the surfaces to combine without damaging the surfaces in the process.

From that point I may add anywhere from 50 to 200 features to the part. There isn't anyway on this earth that I am going to waste my time even thinking about detailing all of those dimensions. No one wants to see those dimensions, measure those dimensions or philosophize about those dimensions. Good luck trying to dimension a bezier surface. The only people that care are the tool maker as they are the ones that have to directly deal with it.

As an Engineer I have to figure out what dimensions are critical to to the fit and function of the part, understand the capability of the tool makers and the manufacturers. Put the few critical dimensions on the drawing and then capture the rest in a note.

And yes I have many parts where changing a feature by 0.001mm will break the part. Not really by my doing, but because I have to start with poor surfaces.

That said a majority of Americans own something that I had direct design input on.
 
If I were to send a drawing that was not 100% detailedto three differentmanufacturers, I would receive three totally different parts back. We have tried using "approximately as shown" for a fewnon-critical featuresand it had terrible results. It is amazing how many different variations of "approximately" people can come up with.


You stated: "No one wants to see those dimensions, measure those dimensions" ? Do you spend hundreds of thousands of $ on tooling, then make the parts, then build a car, then wonder why the car excelerates on its own? THEN measure the damage to see why it crashed?


All of my dimensions are critical. If my parts aren't right, bad things happen.
 
Dan,


I would assume you use a lot of GD&T to describe your design intent. Am I right in this assumption?


If that is the case, a minimally dimensioned drawing would not be practical or plausiblefor you.


For the type of work that I do I can use minimally dimensioned deliverables as my parts lend themselves well to it. MDD's may not be the best fit for every situation.
Edited by: Richh
 
I use GD&T when and where applicable. GD&T is not required in a lot of my instances. Ican not leave any features undefined, ambiguous, or open for interpretation. MDD has notgiven me the results I needed in the past.


Regards, Dan
 
I believe the modeled (shown) dimensions do define the part and are critical in passing information to those who see the part down the road. When a part is sent without a drawing for reference or quote the only dimensions available are those on the part.


Additionally, created dimensionsmay not capture appropriate tolerancing schemes. Many of the part/drawing sets that use created dimensions do so because the part is modeled poorly in the first place.


If there are dimensions that should be referenced though not modeled then they can be added/created as reference dimensions: that is what created dimensions are anyway, are they not?


I push my student to create models with dimensions that define the design and that different dimensioning schemes actually define different parts.
 
I have run into problems with using driving dimensions in the drawing. This is due to setting the number of decimal places in order to define tolerances. By changing the number of decimal places, the actual dimension is then rounded down or up resulting in the size of the part changing. The real problem showed up in the assembly where the part was used because the assembly constraints then failed. For that reason, I always use created dimensions.
 
If the model was designed/modeled at MMC, and then you modified your tolerances to reflect machining boundaries, wouldn't that keep your assembly from crashing? Just guessing here.


I have had models regenerate becausemy choice of tolerance rounded up/down, but it never caused my assembly constraints to fail.


Is it possible thatPro actually did you a favor by pointing out the fact that your tolerance stack may have been whacked?
 
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