Printing Dimensions Drawings of Parts

james_alford

I have created several parts that build up into a clock and wish to print out drawings of them with the dimensions showing.

I can print drawings of sketches with dimensions on, but this only shows one face. I can produce drawings of parts, showing all views, but these have no dimensions showing, unless I manually add them all again.

Is there a way to produce drawings of the parts from all views with dimensions, other than by adding the dimensions onto a drawing again, having already defined them in the original creation of the part?

Regards,

James.

brian_brady

Regrettably not yet. I starting asking for the ability to populate drawings with sketch and extrude dimensions about 6 months ago. Like I said back then, if you model with design intent in mind, you should not lose all of that work and have to duplicate effort while making 2D drawings. In a design department, the lowest paid and greenest designers do the detailing and do you really want to trust them to put the correct dimensions on your drawings to maintain design intent. Onshape needs to implement this soon if drawings are going to be taken seriously.

james_alford

Brian,

Thank you for your reply.

This, for me, is a real limitation and frustration. I have in the region of 40 parts for which I wish to produce drawings to use in a workshop. Ho, hum, a few more evenings work to go, still.

On the bright side, at least I have not been blind and missed something that is actually obvious.

Regards,

James.

NeilCooke

Hi @james_alford

In general, designers and manufacturers require different information - most of the time the dimensions added to sketches represent design intent (such as, this hole should be X mm away from this slot), but the manufacturing people require dimensions from a specific datum, plus tolerances, GD&T etc. Years of experience with engineering and manufacturing companies has shown us that they prefer not to use the model dimensions in the drawing and prefer to detail the drawings separately, as the information required is different.

Doesn't help you in this situation, but that is the reason.

brian_brady

Funny, because to me (and the other design/manufacturing faculty I've talked to about this same topic) design intent is what manufacturing must make a part to and quality control must inspect. There is no reason to specify design intent in a model only to have manufacturing or quality control do something completely different. The best way to ensure your design intent is carried out is to make prints and QC documents directly from the design intent. Are there exceptions where you can only design in a particular way due to the tools you have? Yes, but only until the tool is updated to support your needs. The rest of the time I believe you should design a part the way you need it made/inspected.

Will/can it take a little longer and more thought to model this way? Sure, until you start to think about intent as more than just what you hope can be made but what and how you know it can be made. From my experience in manufacturing and learning from mentors who spent many more years doing there than I, if you design something that cannot me made or inspected, the design isn't worth much. As a side note, if you put a dimension/tolerance on a part that cannot be inspected, there is no reason to waste your time putting it on to begin with.

I agree that manufacturing needs datums, tolerances, and GD&T. That is why each of these must be captured in the design intent and Onshape needs to eventually get to where they do or else they will never be a serious design and manufacturing tool. I want Onshape to be a serious tool, because I think what they are doing it is the future of CAD.

NeilCooke

Hi Brian,

The question really comes down to "What is design intent?" Design intent is completely different to manufacturing and inspection "intent".

Design intent is things like patterns, midpoints, offsets, virtual sharps, variables, etc. that you use during design to specify what is important to make the design work as intended. If you subsequently need to make a change to your design, you expect these intentions to be respected. That is why parametric feature based CAD systems are so popular. Manufacturing and inspection is about creating a part that can be kept in tolerance, is repeatable, and can be produced as cheaply as possible. 

In my experience, I've only met a handful of companies who add tolerances to the dimensions on the model and try to dimension it as they would manufacture it. There are some features that would have the same dimensioning scheme and for those they may use the model dimensions, but the majority of the design would be dimensioned and toleranced, to make it easy to manufacture and easy to inspect, on the drawing. Many were also worried about dimensions being accidentally changed on the drawings as well. Don't get me wrong, I would also like to use model dimensions on the drawing, but I think you'll find it's not as widespread as you might think and does not prevent Onshape from being a "serious" design tool. 

It's an interesting topic - maybe some professional users of SolidWorks/Creo/Inventor could weigh in with their experiences/preferences?

Henk_de_Vlaam

I’m an early ProE adopter. As a drawing board draftsmen I started with it at 1990 and still use Creo. I remember the wonderment of making a drawing by arranging projected views generated by the system and “pulling” all the dimensions (at once) with their tolerances into the drawing. That was revolutionary at that time. And I must say, it still is. That’s why I was surprised that 25 years later Onshape was not able to do the latter. 

In my opinion it is a big step backwards, because brian_brady said it already; the dimensions are already there (as sketch dimensions).

In the early days the main purpose of a drawing was to describe the function of parts, but one learned also that dimensioning was important for manufacturing. So there was a kind of a mix of dimension intent. Nowadays the manufacturing dimensions are much less important because CNC machining has become very common and manufacturing dimensions, i.e dimensioning from one side, has become much less relevant.  

In my opinion model dimensioning and dimensions on drawings meet each other over here. Parametric CAD needs dimensions with design intent, that is: changing a dimension does only change the expected geometry and not the unexpected, it should not be a booby trap. As we saw, dimensions on drawings are needed to show the, let's call it, function intent, i.e. the pitch between holes. These dimensions are also important to do the right tolerance calculations. And, guess what, fortunately the parametric dimensioning and drawing dimensions are in general the same.

I know, in practice a lot of people do not pay attention to design and functional dimensioning (which can be very frustrating when editing their objects). NeilCooke probably you focus on them. But also a lot do!  

So please give the latter the possibility to show the model dimensions in the drawing, with their tolerances!

That will make Onshape on this a tool that can stand in the shade of Creo/SW etc. It can compete, when there is also 2-way associativity which I, as senior (former drawing board user), like very much, because most of the time I optimize the models/tolerances via the creation of the drawing.

That’s why Onshape at this moment does not reach the professional level that is needed. For personal use one can accept this imperfection and enjoy the benefits, which I do.

robert_morris

I understand the need to have certain things dimensioned differently for drawings than they are for the design, but as other have pointed out, it would be nice to not have to do the same work twice. 

One thing that SolidWorks has is the ability to mark certain dimensions in a sketch as "Not for Drawing" so that they would not show up there. You could then use those dimensions to enforce design intent, and add other driven dimensions that would transfer to the drawing for "manufacturing intent".

Another option would be to allow the user to just bring over dimensions from individual features/sketches and hide or show only the dimensions that the user selects. SolidWorks has some tools to do things similar to this as well, and it still allowed you to add dimensions manually if you wished to do so.

andy_10

I tend to agree with Brian, Henk and Robert's view,

There are different ways of using 3D packages for design but from my perspective, parts and assemblies are created with necessary constraints which include dimensions. If you know the specific tolerance required for the design intent, this can be captured in the part sketch or updated later as the design evolves. This data can then be brought into the associated drawing at the time of detailing. If there are any adjustments to the dimensions during drawing creation or after, then the work flow of updating is relatively easy, either update the dimension on the drawing or better still update the sketch in the part file within the assembly so you can review the change impact thoroughly.

Also, the controlled 'engineering' drawing is what we issue to the machine shop or subcontractor to make the part(s). If a machinist wishes to add dimensions or machine a part in a certain way then so be it but, the drawing created by the design engineer is what the machined part(s) will always be inspected to.

michael3424

I'm often the guy that machines or manufactures the things that I design and I usually do parts design with an eye as to how the part will be made.  For me, it would be quite useful to have a drawing initially populated with the driving part dimensions.  GeoMagic Design, my prior CAD program, allowed this as an option - could this not also be made an option in Onshape?