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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.
Relationships and dimensions are what take simple sketch entities and define it into the design you're working on. Relations can control size, location, and equality between sketch elements. And dimension can control angles, physical shape, and the distance between elements or the origin. Let's take a look. I have a sketch open on the top plane. And I have a few different examples here laid out on the screen. First things first, let's take a look at the two lines over here. So I click on the first line here. As soon as I let go of the left mouse button I get a couple options. And notice these are context sensitive.
I only have one line selected, so I only have two options. One I can make it horizontal, or two I can make it vertical. And then finally I can make it fix, and fix just means if I click on it, it just can't move anywhere, it's just stuck where it is. So I don't normally want to use that one, so turn that off. And notice how I did that, and how I got deleted that? Go back, just click on the green box and hit Delete on your keyboard, or you can right-click on the green box. And choose Delete from the Menu. Next if I choose two lines, this line here, hold on Ctrl, slip the next line, next door to it. I've got a lot more options.
So I can say these lines are horizontal, they're vertical, they're co-linear, they're perpendicular, they're parallel, or they're equal. In this case, let's try out parallel. Wherever they are, they happen to be parallel. And if I grab one, I can move it around. Notice they operate as a team now. They're both parallel no matter where they are. And I can move things around, I can still change the length. If I want to make them the same length, I could also add a secondary relationship. Choose both of the lines by holding down Ctrl, and I'll say Equal. Now they're parallel and they're equal. Notice now they are not spinning around. But what I can do is, I can use that little fix icon.
So click on the tip, not the whole line itself, but one of the points on either end, and choose Fixed. Now I have a fixed dimension. If that point doesn't move, then these points here will move around. So it makes it so it could actually simulate some motion inside of my sketch and see how things actually work and layout. Down here, I can choose these lines here. Choose both of those lines. I can say these lines are for instance co-linear. And then put them on top of each other. I can drag it out. And you can still see the point here. And they can be separate lines, or they can be on top of each other. As long as they're co-linear, they all operate as a team.
And there's this little dashed line showing that those two lines are co-linear. In fact, you can even bring this point, and drop it on top of that point there, and that adds a coincident relationship. And now those two points, it's two separate lines, but they're still connected together in a co-linear fashion. Up here you got a couple of circles. Go ahead and choose both the circles by holding Ctrl. As soon as I let go of those circles, I could say these circles are co-radial, or they're tangent to each other, or they're concentric. Let's try all three. First one, co-radial. That just puts them exactly the same as one circle on top of the other, which is really not what we probably want to do in this case, but it does put those two circles exactly on top of each other.
Hit Undo to bring it back. Choose them both again. This time, I'm going to say, these are tangent, so that means they're touching each other. And I can roll this thing around. It maintains a tangency. And, it's a nice way to add the tangency. If you don't like it, you can always delete the tangency. Hit Delete on your keyboard, take it off, now you can move it back away. Select them both again. This time, choose Concentric. Now you have one circle inside the other one. And wherever they move, they'll move as a team. You can adjust different things here. And when you have a couple of circles like this. When we add dimensions, you can add a dimension by choosing the inside circle and placing a dimension, maybe 1 inch.
You can also dimension from the inside circle to the outside circle. Maybe a quarter inch. And I'm adding those dimensions by clicking in the first circle, then choosing the second circle, and then finally, choosing where I would like to place the dimension. And notice, I already have the dimension placed. So if I choose this one, it's going to say, hey, you're doing something wrong here. Notice everything turns yellow, and you're saying, hey. You've already placed a dimension on that sketch. And you'll already defined it as a quarter of an inch. Do you want to add it again? So it's asking you a question. Make this dimension driven? Driven just means, it's just a reference dimension. It doesn't actually control the design.
Or you can maintain it driving dimension, and it'll actually cause an error in the sketch. So I make it driven. Notice it turns grey, and the other ones turn black. So if I change the dimension here to become 0.375, it automatically updates as well, because it's just a reference dimension. However, if I were to go back and add a dimension from here to here. And I said, hey, I actually want to make this a driving dimension, click OK. Now, what happens is, this whole thing says, it's unsolvable, because it doesn't know, is it use, supposed to use this dimension here. Or this dimension here, because it's giving the same information, by both of them.
So what you can do is delete either one of them. And then it's back to being happy. Notice all the lines are still blue, though, because they don't know where they are. So to solve that problem, we either need to place this on the origin, or add a relationship to where it is in space. One of the great ways to do that is using the Center Line tool. So, I'm going to make a line from here and bring it right up to the top. And now wherever I drag this thing, I've got a couple of lines that attach me to the origin. You can add a dimension by clicking the line, I'll say 0.75. And, over here, I'll say this is going to be 2.5. Notice as soon as I do that, everything turns black and it knows exactly where it is, because we always want to relate our sketches to the origin.
So they know where they are in space. Continuing on, let's go ahead and grab the Smart Dimension tool. And here's an angle. I want to define the angle. To do that, you're just going to choose the first line And then again choose the second line. And then you're going to place the dimension. However dimension tool is dependent upon where you place it in relationship to the angle. So over here, I've got 30 degrees or 30.96 degrees. As I move this around the circle notice that it's the same angle, it's just showing you how it would place the dimension differently. Same thing over here. Same thing down here. So as you move around that circle, it keeps changing, how it's going to place the dimension.
In this case here I just want to place it inside. I'll type in 30. Click OK and adjust the dimension. These lines can still move, but it is now defined as 30 degrees. So I can't change the angle. I can still just move things around. So again I'd want to tie that into the origin or tie that into something else. And finally, I've got this rectangle here, and I want to add a few dimesions to that. To do so, I'm going to go ahead and choose the Dimensioning tool. There's a couple of different ways to use the Dimensioning tool. Number one is, I could just choose a line itself and put a dimension. Which is fine, however, what happens if it was not a full line? What if that line didn't continue the full length? For instance, I'm going to give you a sneak preview here on the Sketch Fill It tool, and I'm going to fill these corners.
They're going to have a rounded corner to those four corners. Okay, I'm going to increase the size. Now, in this case here, if I use a Smart Dimension tool, it only dimensions that length. So, I'll take 2.0, its only dimension from here to here. It's not the full length of the shape. It's really not what I want. So go ahead and delete that. Grab the Dimensioning tool. This time, I'm going to dimension from the left-hand side all the way over to the right-hand side, and then third, I'm going to place the dimension. That's called a 3 pick dimension. I can type in, 2.5 and place the dimension. I always try to use a 3 click dimension because it allows me to radius the corners or make other changes, and it doesn't affect that filed dimension.
Adding and using relations can be a huge time saver and makes your sketches easier to update and simpler to understand. Relationships and dimensions are used throughout Solidworks. And an understanding of how they work is extremely important.
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