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SolidWorks is the world leader in 3D software for product development and design. Start creating manufacturing-ready parts and assemblies, as well as detailed drawings and bills of materials. In this course, author Gabriel Corbett shows how to create 2D sketches that will become the basis for your 3D models. You'll use the Extrude and Revolve tools to turn 2D sketches into 3D parts, then create more complex geometry with sweep and lofts. Then learn how to use the cut features to remove material and shape parts, and use mirroring, patterning, and scaling to modify parts. Next, you'll combine parts into movable assemblies and subassemblies. Finally, you'll create accurately annotated drawings, complete with itemized bills of materials that relate the final parts and assemblies to a manufacturer.
In SolidWorks, the size and features are defined in the model. Therefore to add dimensions, we just need to define what values, and where to show them. SolidWorks has an autodimension command as well, that can do a lot of this for us. The tools are straightforward. However, what is not straightforward is understanding what and where to tolerance. There's a lot that goes into this, and we'll cover the basics. To get started, notice, I've got 18.1-1 opened up, the drawing of that part. And you can see here, I'm looking at the top view. And first thing's first, I want to get started with using the regular Smart Dimensioning tool.
I also want to point out, before we get started, if you click on this little drop-down arrow on the Smart Dimensioning tool, we have a whole bunch of different dimensioning things we can use here. The Smart Dimension kind of just automatically picks one of these for us, so I'm going to go ahead and use that. But you can specifically choose, for instance, a horizontal dimension or a vertical dimension or a baseline ordinate. And we're going to be getting into a lot of these. Starting off, smart dimension. Let's get started. Okay. The first scheme we're going to be using is called a baseline dimensioning scheme. And what that means is we're going to have to choose a baseline. A baseline's just a choose a line in the part. In this case here, this is going to be my baseline for the horizontal.
And this is my baseline here for the vertical. So starting off, pick this line here. Come over here and pick one of the features like this circle here. And then I'm going to come down and place where I want that dimension to be. Pretty simple. The dimension is already defined from the solid model. So I don't have to go and type anything in here. It's just referencing the solid model, and putting the dimension on my drawing. Pretty easy. Select this line again. This time select anywhere on the outside edge of the hole. Or the inside hole. Doesn't really matter. Again, place the dimension. Over here, this next hole from there to there, dimension, great.
From this line to this arc, which will then show us the center point of that arc. Go ahead place the dimension. If you want to dimension these lines up here at the top, you can still choose that same baseline and then just place the dimension on the upper side of the model. Again, choose a line, to the leather line, place the dimension. Start from this line here, dimension of this line here, place the dimension. So everything is always starting from that same baseline. That's the key. We always have to go back to the original line, and every dimension has to start from there. Start from here, dimension to a hole. Place the dimension.
Start from here, go to the end of the part, place the dimension. You can see this dimension scheme is quite easy to work with. However, if we have a lot of features, you can really stack up quite a few dimensions and sometimes it can get a little bit unwieldy, when you have a hundred dimensions in a row underneath a part or above a part. So we might want to look at some other dimension schemes in that situation. The next one I'm going to work on is doing that vertical baseline. So back to the Smart Dimensioning tool. Click on this bottom line here and then again to maybe the first hole. There's my first dimension from that line to this second hole.
From that line to the third hole. And once you have them, obviously you can move these things around, make them look a little nicer, right? I can place the dimensions here. I can align them so it looks a little more clean and you can place dimensions below the parts if you need to. You can place them inside the parts. You can move everything around getting so it's looking nice and uniform. And that's the key. Now if I want to change the tolerance or the amount of decimal places I'm showing, I can easily do that by clicking on a dimension. Coming over here to the dimensioning tool bar and I can choose what type of precision I'd like to add. So I can add like a basic or bilateral or symmetric.
So, for instance if I use a bilateral it'll change and add that to this dimension right away and I can type in oh, I want to have this to be plus ten, but minus nothing. And I can determine how many decimal places I'd like to add so I could say I want, two decimal places. And that will round that down or I can add more if you want but, in general you don't want to add more decimal places than you need to fully define the part the way it needs to be. You don't want to add, oh I can add this many decimal places. Sure you can, but you don't want to do that 'cause it's going to make the cost of your part much, much higher if somebody's tryna actually manufacture this to that level of precision.
So you want to make it as loose as you can in order to fully satisfy the requirements of the part. That's kind of the key there. So cut this back to two place decimals. Looks great and you probably change the other ones. Anyways, that's what we call baseline dimension scheme. The next one I'm going to do is what we call a chain dimension. So I'll just go ahead and delete these dimensions here. I'm just deleting them by running a box around them and hitting delete on my keyboard. And you can just pick individual ones as well. Just delete, delete, delete. Okay, now we're going to jump into what we call the chain dimension.
The chain dimension back up here, is just really how you choose the entities. So from the first entity here, I'm going to dimension to this first hole. From the bottom line here, I'm going to dimension to this first hole. Again, same hole. Now, instead of dimensioning this way or that way, I'm going to dimension from that hole to the next hole. And then from that hole to the next hole, and again from that hole again to the next hole. So what you see here is one is reliant on the previous dimension, so what happens is is As we start stacking these up, we get what's called a tolerant stack up.
So if these are plus or minus five thousandth of an inch, each one, and when you get down to the end we've added five thousandths, ten thousandths, fifteen thousandths of tolerance between the first hole and the last hole. Where as if you were to use a regular baseline dimension, like from here to the last hole, that would by control plus or minus five thousands of an inch from this line to that hole. So you have to really choose and see what's important in your design. In this care here, if it's more important to have a 0.6 between these holes than it is to have the dimension from the edge than this might make sense.
But a lot of times, chain dimensions can get you in trouble because that last hole can be way out of tolerance from where the first hole is, and so on. So, keep in mind how your part will be used at the end of the day, what's important to the design. And a lot of times, you'll end up coming with some type of dimension scheme that uses a combination of both baseline and chain dimensions. And that's what I'm going to show you next. Go ahead and delete these, and what we're going to do here is, we're going to dimension from the bottom edge to this first hole. So that's a baseline dimension. Then we'll do a chain dimension from here up to the next, and then I'm going to continue going back to this first hole.
So then that will become my new baseline. So I'm going to dimension each one of these holes based upon that first hole. And the reason I want to do that is, I wa-, I want to make sure that these holes are tightly held in tolerance. However, I might want to loosen up what that tolerance is to the edge of the part. So over here, instead of 0.350, let's change that to maybe 0.35. So I have a little bit looser tolerance, plus or minus ten thousandths from the first hole to the edge, but then from that first hole I'm holding plus or minus five to all the other holes. It's a nice way to use a combination of both, and gives, it's a nice space saver as well.
Dimensioning and Tolerancing is a class in itself. We touch on the basics in this movie, however, this is definitely an area that will require a bit more study to be great.
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