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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.
Almost all features in SolidWorks start with a sketch. Sketching correctly and efficiently is a key to being a proficient designer. To get started, let's go ahead and choose one of the three fundamental planes. I can see have the front plane, the top plane, and the right plane. I'm going to go ahead and choose the top plane. Click on the Sketch icon. And starts a brand new sketch on that plane. Notice I have the origin in the center of my part, and that's really important. We always want to tie into the origin. To get started with, under the Sketch tab up here, we've got a bunch of tools we're going to be using in sketching.
The very first one is Exit Sketch, so when we're done with our sketch, we're going to click on that and it's going to take us out of that sketch environment. Number two icon here is the Sketch, or, Smart Dimension. And we're going to be adding dimensions as soon as we actually have some geometry to sketch upon. After that, we have a whole bunch of other features that we're really not going to be touching on to much right away, but we will be in the course. At first, the only two tools we really need are the Line and the Circle tools. And in this movie, we'll just be using the line command. So, go ahead up here, and grab the Line tool. And by the way, notice as I mouse over it, it gives me a little heads up display showing me that L turns on the line command.
So if you ever want to be. In the sketch environment in turn the line command, just hit L on your keyboard or hit L again to turn it off. So now that I have the line command, I have two different methods for drawling lines. Number one is called the click, click method and number two is called the click and drag method. So let's try it out. First things first, click one and notice as soon as I click, the line is now attached to the tip of my cursor. When I move or Swing around, you can see that the length of the line is now displayed. It's at 2.61 for instance as you move it around here. As soon as I get to a vertical orientation, notice that it shows me the angle. So, I'm at 90 degrees and notice that little yellow box.
That yellow box is showing me that if I were to click right now, it would add an automatic relationship showing that this line is a vertical line. I can get the same thing if I go over here to the 45 or the 135. It'll show me what angle I'm at. Or if I come over here to the horizontal, notice I get that little yellow box again, it's going to say, hey, you're at a horizontal relationship. And if I were to click, it would automatically lock that line into being horizontal. If I click over here at an arbitrary location, Close to six inches. Notice as I click, now there's this little yellow helper line showing me what is continuing to be co-linear or perpendicular relationship.
And it also gives me the heads-up display again, of how long that line is. And this command is going to continue on until I hit escape or cancel out of the command. In this case, I'm not going to click on any one of the little helper lines, I'm just going to click out in space here. And again, it, it just keeps going. You get the helper lines every time you click. And, just go ahead and click over here. And then notice as I get close to the closings box off, I come over here to the very beginning point. Notice that gives me that little circle inside of a circle. Which means it's concentric, or coincident to the starting point. Click OK.
And, notice that command automatically gets turned off now because I've completed one enclosed shape. Okay, when you're happy with the line command, you can either click on OK, or you can escape to turn that off. Now, that I've got these lines on my screen, I'm trying to create a rectangle and I'm really having a hard time here, right? So, doesn't quite look like what I'm looking for. So I can click on the corners, and I can drag everything around a little bit. I can click on the lines themselves, I can drag them up and down, but I really don't have quite a rectangle. So I might want to move things around to kind of get it more in the orientation of a rectangle, but it's going to be hard for me to get a perfect rectangle.
Without actually adding some other type of relationships or some other constraints onto this shape. So, first things first, let's go and add our very first relationships. So, relationship is something like a perpendicularity, or equal, or parallel. So, to create this shape into a real rectangle, I need to add a few of those things. So you think back to your geometry classes, you might remember that create a rectangle you need parallel lines. And click on this line here. You can hold down Control on the keyboard, pick this other line over here.
And as soon as I let go of Control, I get these little available relationships. So I can say these lines are horizontal. They're vertical. They are colinear, perpendicular, parallel, equal, or fixed. Notice I also get those exact same relationships over here on the left hand side of the screen. So I can say these lines are parallel, and notice what happens. They become parallel, and it gives this little green box showing that. These two lines are parallel. And notice if I mouse over either one of those lines or the box there it shows the two lines that are involved in that parallel relationship.
And notice that zero next to each one. The zero means nothing more than to match a zero with another zero. Same thing if I do it again. If I say this line here. Hold down control on the keyboard. Pick this line here. As soon as I let go of control. I get the little heads up box. I can click on Parallel, and notice these ones have one and one. What that means, if I were to delete this one. Click on it, hit Delete on your keyboard. It deletes both of them, and that shows they're back there. If wasn't what you would like to do, click on Undo, and it brings them back. Okay. So the question is, is do we have a rectangle now? No.
We have a parallelogram right now so what we'd like to do is make them a real rectangle. But what I need is to save this line here, hold down Control, this line here and I'll say, let's make these perpendicular. Now I have a rectangle. However, it's still not perfect. Maybe what we need to do is square this thing up. So maybe a line here and say this line is horizontal. Now that it's looking better, the only thing we have that's missing is we have the shape, but we don't have the size or the location of the rectangle. So first things first, we have this origin here and we generally always want to tie into the origin whenever we're working in a sketch.
So I can drag the corner, right over here and snap it right on top of the origin. Notice, as soon as I do that, I get these black lines, here. Everything else is blue and now they're black. We have three different colors of lines. Number one, a blue line, means it's undefined or under defined. A black line means it's fully defined and knows exactly where it is. And a yellow or red line means that it's got errors or, or cautions that is causing issues for us. Okay, first things first. Let's go ahead and finish off this rectangle. So let's go ahead and grab the Smart Dimension tool.
Grab one of the lines, click where you want to place the dimension, type in 6.0, again when you have the dimension tool. You can click on the line itself and and a second click is going to be where you want to place the dimension, in this case here 3.0 type it in and you just hit enter and replace the dimension. Notice that everything turned black, we're ready to go. Let's go ahead up to features. Let's go up to extrude. Let's drag this up. Let's type in a number of 2.0. Click on Okay. And there we go. We created a brick.
Sketching is the most important aspect of design and is the key to good SolidWorks features. Take the time to think through your sketches and develop simple and effective layouts. Look for symmetry using construction geometry and adder relationships.
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