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?
I would think if you went to the assembly level and created a relation
between parameters on separate parts they would be tied in Pro/E. And
when you create drawings, both would dimension like any other parameter.
Are you dealing with some other package than Pro/E? -meld
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
For example, you can create sketched features in a protrusion that have
'symmetry' about a construction line. The 'shown' dimensions will only
show the dimension between the features, not the implied 1/2 dimension
to the symmetry feature.
I think dakeb is saying that generated dimension (those created indirectly
a calculation in a relation) were being banned. Only those directly created in
model would be allowed, meaning no loss of parametrics, but certainly some loss
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
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
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 would think if you went to the assembly level and created a relation
: between parameters on separate parts they would be tied in Pro/E. And
: when you create drawings, both would dimension like any other parameter.
: Are you dealing with some other package than Pro/E? -meld
: dakeb wrote:
: > 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?
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?
David Janes wrote:
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
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
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.
Polytechforum.com is a website by engineers for engineers. It is not affiliated with any of manufacturers or vendors discussed here.
All logos and trade names are the property of their respective owners.