We have been asked to only use shown dimensions on drawings. The implication of this is that every feature needs to be dimensioned in the model, not the drawing. That means when you put holes in one part, you can't make the holes in the mating part parametric to it, you have to dimension each part separately or the dimensions won't show up in the drawing. Losing parametric relations seems to defeat the object of a parametric CAD package. How do others address this issue?
No, it's ProE. Yes, you can make dimension relations between parts which will allow the dimensions to show up on the drawings, but that is so much extra work at the modelling stage and moves the design intent effectively from the model to a text file (which I dislike).
I have had many responses from the user community on this, and the vast majority advise use of dimensions on created drawings for two main reasons (there are many other minor ones too):-
1) Loss of parametric capability (unless you use relations)
2) Design intent of a part is different from the manufacturing intent of a part. Drawings are based on the manufacturing intent of a single part, but parts are based on the design intent of the whole assembly. The dimensioning of a part drawing should never drive the assembly design intent.
I have experimented going in the other direction when using SW.
I used to create all the dimensions on the drawing instead of using shown part dimensions, because I did exactly what you are doing. I had many 'in context' assembly references for part features. In Pro-E I have found that 'in context' assembly features are a nightmare, and need a very specific regeneration of the components in the assembly to work porperly, so I abandoned the concept.
I would agree also with an earlier post that the manufacturing requirements may differ from the design intent or require dimensioning differently.
For example, you can create sketched features > No, it's ProE. Yes, you can make dimension relations between parts which
I think dakeb is saying that generated dimension (those created indirectly through a calculation in a relation) were being banned. Only those directly created in the model would be allowed, meaning no loss of parametrics, but certainly some loss of sophistication, top down modelling and more advanced design intent. The whole discussion on skeleton models which began with a post from Andrea Willans covers many of the advanced (and indirect) modelling techniques which don't fall in the fanatical, dogmatic approach that requires 100% shown dimensions in drawings.
It would be ineteresting hear the reasoning behind this dictum. The only rationale I've heard is to facilitate people with little or no Pro/e experience to change drawings, to let your former board drafters (who universally hate Pro/e) to monkey with the prints without having to see those nasty models and figure out those oh-sooo-complicated relations. Poor babies should have been put to pasture long ago. But why cripple Pro/e to stroke such people? Is there a legitimate reason to demand 100% shown dimensions in drawings?
I'm with you on this, James. I've heard this many times and generally, if you have model dimensions it is better to show them than to recreate them in the drawing. But when this is being turned into some kind of a rule, an unbendable company-wide policy, it's just plain stupid. If there's any 'golden rule' in engineering, it's that every 'golden rule' has plenty of exceptions. People who make policies like that simply mistrust their engineers. Their efforts would have been better spent trying to find better engineers or to educate ones they have.
Wow - interesting points in this thread... I do agree that moving a lot of things into relations does seem to degrade to basically editing a bunch of text. It seems fairly often that I write relations (just on piece parts) and then forget that they are there and a couple taps on the parameter before I go... oh yeah!
This whole topic of allowing the power users to really use the software without totally confusing the less skilled users in a company could probably have books written about it. I bet behind the "dictum" is some horror story where managment said ... let's not go there again! I keep asking folks if we should "chart this failure" so as to avoid it next time and so far I've got no takers.
The manufacturing intent vs. design intent topic is a deep one too. OK I've heard the argument that how something is built in Pro/E is NOT usually how it gets toleranced... is this the same discussion? Making someone think about the best tolerancing method at the same time as most flexible for modeling IS over constraining... But this isn't a problem for companies with lots of experienced Pro/E users and no misguided dictums is it?
"meld_b" wrote in message news: snipped-for-privacy@yahoo.com...
One way to cope with that is do modify the dimension text to show a 'Relation Driven' note when you attempt to modify it. However, this note will then show up in the drawing when you show the above dimension. Usually, when I am building a moving assembly that has, for example, linear slides and a leadscrew, I'd make an assembly datum plane named 'Stroke' or some such, put a note into the dimension driving this plane with critical points (like 'Total stroke 0 to 12", actual - .25 to 11.75) to remind me what the range of motion of my assembly is, then create relationships driving the linear slide carriages and the nut of a leadscrew using the 'Stroke's position, and maybe add 'Relation Driven' note into the respective dimensions of the linear slide and leadscrew subassemblies. None of these dimensions are later shown on the drawings, but putting notes into them helps a lot when fine-tuning or modifying the assembly. On the other hand, when I need to bolt one part in an assembly to another I simply create dimensioned holes in one part and then make holes in the second one using the first part's holes as references. This, of course, makes it necessary to create dimensions for holes in the second part in the drawing: there is nothing to show/erase. Using this method saves a lot of time at the design stage: linked features move together when the assembly is modified and there is no need to worry about mounting holes in one part 'walking away' from their corresponding hole pattern in the other one. In my opinion, this advantage by far outweighs the additional time spent creating a few dimensions at the detailing stage. The 'Model dimensions only' fanatics are, in my opinion, undermining one of the most useful features of Pro/E (or any other associative 3D package).
Dimensioning is a very basic skill. An engineer and even a drafter who do not know how to dimension depending on the manufacturing method and design intent, and are not proficient with their CAD package's dimensioning tools are in a desperate need of remedial training. Until they acquire these skills they are a disaster waiting to happen regardless of what their management does to 'dumb down' the design process.
Regardless of how skilled the designer is, there still are occasions when the way you model the part and the way it needs to be dimensioned for machining are not the same. For instance, you are modeling a plate with a bolt pattern that needs to be symmetrical about that plate's centerline. Naturally, the bolt pattern's dimensions in the model are created to reflect that. Now the drawing is out on the shop floor. How do you think would the machinist like it to be dimensioned? Simple: he would want you to set one corner of your plate as zero and dimension all features from this corner. Why? Because he will then zero the DRO unit of his mill on this corner and will easily and accurately dial every hole in from this zero point. If you just 'Show' the symmetrical dimensions from your model, the machinist will probably spend some time recalculating all of them from some corner of the plate anyway. Additional time will be spent, not to mention the possibility of him making an error in his calculations and scrapping the part. On the other hand, if you model the plate with the dimensions created the way the machinist wants them, nothing really enforces the bolt pattern's symmetry and if you (or somebody else) modify the assembly later, there is a very real chance that the bolt pattern's symmetry will be lost. The only way to avoid this in this situation is for you (and everybody else who will at any time be modifying your assembly) to manually verify that the symmetry is still there after the modifications. Again, additional time is spent and the possibility of human error is high. Now, in such situation I would simply model the part with symmetry enforced by dimensions and sketcher constraints, and then create ordinate dimensions from the part's corner in the drawing mode. The additional time spent will be minimal, the possibility of human error during recalculation - zero, and both my design intent requirements and the machinist's requirements will be satisfied. By the way, I find quite often that people (especially management types) get confused by terminology: they somehow tend to assume that 'parametric' and 'associative' (read: good) only pertain to model dimensions, and that dimensions created in the drawings are 'non-parametric' and 'non-associative' (read: bad). Let's keep in mind that this is not true: the dimensions created in the drawing mode update with model changes just as reliably as the actual model dimensions. If the dimensioned features are deleted in the model, their dimensions created in the drawing fail during the next regen and have to be deleted. I could come up with quite a few situations where design intent requires one dimensioning scheme in the model, and manufacturing requirements call for a different dimensioning scheme on a drawing, but this has already become a long rant. Let's just say that until engineering drawings go the way of the drafting board and all machining is done directly from the model, dimensions created in the drawing will be necessary and trying to ban them will only waste time and money and create screwups instead of eliminating them.
This has been an interesting topic. Obviously, both types of dimensions are necessary. With the discussion of driver and inserted dimensions, has anyone come upon a config option or dtl option which would allow the designer to distinguish between model and drawing dimensions easily such as a font or color change? This option should be easily switchable since once the drawing is plotted, the dimensions should all look the same but it could save time looking for a driver during design.
I say 'Show' the dimensions that you can utilize in the drawing effectively, and 'Create' the rest. It really does require a combination of both dimension types, but in Assembly drawings you obviously have to 'Create' almost all of the dimensions that reference entities of two different components. Subtractive Assembly features would be an exception to this. One thing to watch out for when 'Creating' driven dimensions in drawings is this. It *is* possible to inadvertently select a dimension reference entity that is some small distance from the intended dimension reference entity. Meaning a solid edge that doesn't lie in the same plane as the intended dimension reference entity and cannot be seen in a 'No Hidden' drawing view environment. For people working in the electronics industry this little mistake can be costly. We're talking about people working with incredibly tight tolerances in many cases.
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