I can't help you with that. I abandoned using model dims years ago. It seemed like it took me just as long, or longer, to move them around to where I wanted, and I don't want to have to worry about how I'm going to do the drawing while modeling.
Michael Lunney wrote:
My company has a best practices standard of pulling dimensions and tolerances into the drawing using Model Items. What, in your opinion, is the benefit of using Model Items over using the Smart Dimension tool in the drawing?
I understand that using model items would require the model to be created in such a way to reflect design intent, and that's not a bad thing, but I've worked for other companies who dimension the drawing using the Smart Dimension tool, regardless of how the model was created and that seemed to work out okay.
It takes longer (time is money) to add more than just nominal dimensions to the model and pull them into the drawing than to create a dimension scheme and capture the design intent in the drawing alone. I'm wondering how this is value added to our company. If I'm missing something please clue me in!
Two 'benefits' I can think of:
- You an change the dimension/tolerance in the drawing and the model updates accordingly.
- Some dimensions behave better when they are imported. I notice this mostly with things like foreshortening, or dragging dimensions from one view to another view such as a detail view.
That being said, I use both imported and manually added dimensions. After nearly 20 years of SOLIDWORKS use, there is an mental dividing line in my brain that tells me when a model is sufficiently complex that importing will be more work than manually adding dimensions. I also use a lot of ordinate dimensions (more compact), which I rarely do in the model itself because the ordinate dimensions would have to span multiple features and sketches.
As Glenn Schroeder stated, they do sometimes take longer to move around. However, I do believe in inserting those with tolerances attached because if I change my mind on the tolerance and fix it in the drawing it populates back to the model.
I think this ultimately depends a lot on what you're doing in SolidWorks. For bespoke machinery design, part models are created in such a way as to make them easy to work with in the context of the assembly. There may be midpoint relations, references to sketch geometry, or even in-context references to the assembly. Many of the parameters that end up defining the shape are completely inappropriate/invalid/invisible in the drawing of the part. Smart dimensions are applied in the drawing and defined in such a way as to allow for the most efficient manufacture of the part without sacrificing function.
I tend to create dimensions on my drawings rather than bring in model items. When I used Pro/E (now known as Creo), I tended to bring in about half my dimensions from the model and create the other half on the drawing. I still haven't tried a suggestion that might make bringing model items in easier, but mostly I find it frustrating if I have a complex part. By the time I find the dimension I want to import from my model, usually, I could have recreated it several times over.
Design intent and dimensioning/tolerancing intent may be different. For example, I am very likely to constrain things in my model around a centerline. I would very rarely dimension these same features about a theoretical centerline. I balance the needs of the design with the practicalities of inspecting to a drawing. Another similar situation, I may want holes that are all a certain distance from the outer edges of my part. I can dimension my sketch that way, but I wouldn't dimension my drawing that way since the tolerance stack up would be higher than if the holes were dimensioned from each other.
Edit with additional info:
If you need to do ordinate dimensions, you either have to do them all in one feature to import into your drawing or you end up with multiple zero locations.
I have a drawing I get to do a CN (or ECN, or ECO whatever your company calls it) for because the original person who modeled the part liked ordinate dimensions and showing his dimensions. The part is a square with a hole pattern that is supposed to be centered. The holes are located with ordinate dimensions. We had to change the outer size of the square based on material availability. When the outer size changed, the holes stayed the same distance from the zero edge. We got a couple of them moved so they were centered, but missed a couple. The actual design intent was for the holes to be symmetric about the center. If it has been modeled with design intent and then the ordinate dimensions created, we wouldn't be doing the work on a CN.
I'd like to use them more, but I normally give up because it's taking too long.
I have an ambition to create more drawings using model items with the aim of allowing our joiners to create their own prints.
At present I only have a couple of simple utility models like this diamond pattern generator for nail locations on a door. It's been really useful.
Too funny I was just talking to someone at the company I first started as a designer using Solidworks. (He was kind of a mentor for me for a couple of months). His first piece of advice on drawings was about this very topic.
"If you are going to design and detail your projects, fit whichever scheme works for you. If you are going to design and rely on someone else to detail, or you are detailing someone else's design use the smart dimension.
You do not want a "green" employee or an intern pulling in model dimensions with the ability to change model features by a simple mouse click and a keystroke. We were running DB works file management at the time and you had to check out the assemblies and all of the parts to detail, otherwise it would not rebuild correctly and custom properties would not stick."
(I paraphrased a little as it was almost 10 years ago.)
To this day I use a mixture of both. Since a good chunk of our designs are built in-context traditional dimensions from the model don't always play well together. But if I have an inline rotary shaft with multiple diameters and features, I dimension and tolerance them in the design so I don't lose the overall tolerances I need. So those I pull the model dims in anyways because I already mapped out my fits and everything when I designed the darn thing.
Agreed. Very rarely does it make sense to pull in the model dims. Although, in a perfect world, I would love to always use model dims because of how nice it is to have dims linked within your drawing and be able to edit both ways.
I'll just throw out a little tip for those of you importing model dims to save time arranging your dimensions. If you click drag to select all imported dims,
then hover over this little symbol...
The dimension formatting window will display.
Then click this button in the dimension formatting window This will auto arrange all selected dimensions. It actually does a very good job in my experience.
Several people have mentioned the ability to edit the Part from the Drawing using model dimensions. As far as I'm concerned, that's a drawback, not an advantage. If I make a change to a Part I want to see what it does to the Assembly. Although for people that only work with Parts that would be less of a problem.
Thanks for all your responses. I'm in agreement about using either a combination or the Smart Dim tool on the drawing only. Also, I haven't seen many people here use much GD&T, likely because it makes the project harder to have to put those annotations on the model and pull them in as well.
It is FAR faster for me to capture the design intent of a part on the drawing alone from a nominally dimensioned model.
I'm going to begin a push to relax this requirement a bit. Thanks again for all your help!
This is cool and will definitely help!
I don't consider it a benefit to change a model from a drawing. Open the blinkin' model and change it. Then check all the assemblies where it appears to make sure you didn't break anything. Then update the drawing.
If that's too hard, you're too lazy. Do us a favor and go work for the competition.