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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.
Sweeps allow for the creation of tubes, hoses, wires, and any other shape that has a constant profile formed into a shape. Think of a wire hanger. The wire size stays the same. However, we can form it into any desired shape. The requirements are a profile and a path. Their profile is a shape that is constant. For a hanger, the profile would be the simple circle. The path is the final shape that we want to build. This requires two separate sketches defining both the profile and the path. On the screen here, you can see I've got the first of the sketches done. It's sketch one, and it just defines the path of a little hanger.
The second thing I need to do is create a profile that I'm going to sweep along this path. Now, most of the time, I would start a profile on either the front plane, the top plane, or the right plane. However, I need to start that profile on the end of one of these line segments, so either at the end of this here or the end of the segment here. So that makes it a little bit more difficult. So what we have do, is actually create ourselves, a reference geometry plane. So go up here to reference plane, click on the line itself, and then go ahead and choose the point at the very end. What that does is actually put a point at the very end, of that line segment, so i can nicely draw a circle, to create my profile.
Go ahead click OK, choose that plane. Go to Sketch, start a brand new sketch in this case here I'm going to choose a circle. Come in here draw the circle out let's go ahead and add a dimension, I'm going to type in 0.375 it's going to be one of these classic hangers click OK. And when you're done, exit out of the sketch. I can even hide that plane. Now I see I've got a little circle on a plane. It is perpendicular to the wire path. And that's all I need to get started.
Let's go up to Features. Let's go to Swept Boss or Base. Click OK and notice the little icons. They look exactly about what we have here. We have a little circle along a path and then we have a path. So first things first, let's chose a circle. Now you might be tempted to come out here and choose the circle from the window here, and that will work sometimes, but it's actually a lot better to choose it from the tree. If we expand the tree out here, come over here to sketch two which is the profile. And then come down here to the path which is actually sketch one. As soon as I choose that one, I get a example of exactly what's going to happen here.
You can see the paths intersect a little bit, and click OK, and there's our shape. So we've got that wire hanger we just built out of there. And you just take anything you want to change in that path. You can always go back to that sweep. Jump into the sketch itself, edit the sketch, spin it around, if I want to change that to maybe a quarter inch, exit out, and it automatically updates. So, pretty simple to define wires, hoses, tubing, structural members. A very useful tool. And you could even do some complex things like spinning things around in the path.
If you go back to the Sweep one, click on this, we also have these other options down here. We can follow the path, we can twist along the path, we can keep normal, too. So you can get some pretty, wild things here. We can also look at the alignment. How do you want to define the direction vector? We can add guide curves, just like we could in lofts. And that really starts getting into some very complicated modeling. It's a little bit outside the scope of this course, but I do want to point out that they're available if you want to look into them further. When you're happy with all that, click OK, and we're done with that.
Swept shapes are easy to create as long as you have the correctly defined profile and path. The complexity of this feature is based upon laying out the sketches correctly. Spend the time to think through how you want the shape to be created, and the best way to build planes in their corresponding sketches.
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