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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.
Swept cuts allow for a tool or profile to be used to cut along a path. The creation is almost the same as using a regular sweep, with the addition of something to cut through. I've got three different example here I'm going to go through. The first one is I'm going to have a little cut or tube that actually go through the inside of this part. So what I'm going to do is I'm going to first start off with the path that I want to go through. So I want actually this hole to be on the mid-section of this part, so somewhere between the top and the bottom of the part. In this case here, I can look at the planes I have available, the front plane, the top plane, and the right plane, and none of them really seem to be in the right location.
So let's go ahead and create our own plane. Come up here to Reference Geometry, choose Plane, and I'm going to choose the top surface. And I'll rotate my model around and choose the bottom surface. And by doing that, it places a plane between those two faces. Click OK. And that's what I want to draw on. So I'll go ahead and choose that plane, start a sketch, and press the space bar to look at Normal Two. Then, come up here. And, let's use the Line command. Let's just start, right here, at the bottom edge. Come up. Come over. And come down. I know that I want to add a Fill It to those corners.
So, I'm going to choose the Fill It command. Click on the corner here. Click on the corner there. And, 3/4 inch looks good. Click OK. And, then, I want to make sure I'm centered up. So I'm going to choose the origin. And I'm going to snap to the mid-point. And notice as I go over that line, a little mid-point dot shows up. Click on that and then say, hey this line here, I want to make that vertical. Let's go ahead and add a couple of dimensions from here to here. Let's make it five inches. And from the top to the bottom of the part, let's click and place the dimension, making it 9.0. That is going to be our path. Go ahead and exit out of that sketch.
Now, I'm going to come down here to this face at the bottom of the part. Start a sketch. And what I want to do is choose the circle command. And I'm going to start right in 3-D here, choose that endpoint and I'm going to draw a circle. Jump over to the smart dimension Add a dimension of half inch. And then exit the sketch. So now I have everything I need to create that swept cut. I have the path and I have the profile. And I'm ready to go. So go ahead and jump up to Features. Come over here to Swept Cut. And as far as my profile, I'm going to do a Profile Sweep, and I'm going to choose my profile.
And go ahead and choose it from the tree. I'm going to expand that out. And I'm going to choose sketch nine. And for the path, I'm going to choose sketch eight. There's my two cuts. Click OK. And there it is. It cuts right through the part. And it's a little hard to see, because it's inside, but what you can do is, you can come up here to the section view. Section it in half. Click OK. You can see how that path is cut all the way through the part. And it just takes basically that simple little circle and drives that circle as a cutter all the way through the part following along that path. Click OK, bring it back. Alright, that's example one.
Example two is we're going to take this profile here and we're going to drive that profile all around the outside edge of this part to create a nice, decorative finish. To do that let's go up to Swept Cut. As far as the profile, I'm going to come up here and choose sketch two. As far as the path, I'm going to choose sketch three. And it's just going to take that and just drag it around the outside of the part. Click OK, and there it is. We've created a pretty complicated part now with pretty much a simple sketch and a simple path. But it looks pretty neat. In the final example, what I'm going to do is what's called a Solid Sweep.
So in this case here, I've what I've determined is a end mill, and that N mill is going to be plunging into this part at an angle. This type of cut would be extremely difficult to model otherwise if you weren't using a Solid Sweep. And I'll show you why. First off, come up to Solid Sweep. And this time I'm going to go to Solid Sweep option. And it gives you some heads-up information here as far as what you want to choose for using a Solid Sweep. And what I did was I actually created a separate revolve feature here which I modeled in end mill. I'm going to use that end mill now to cut into the part. So as far as my profile or my tool body, I'm going to choose this end mill.
Which just happens to be a simple rectangle that I rotated around the central axis. And then as far as the path, I'm going to come down here to choose sketch five. Click OK. And you can see what happens. When it cuts down there, it takes that shape and drives it into the part. And if you look at this, if you actually can see a little of a rounding of the backside of where the end mill was. And you can see when it's down to the bottom, it has this nice round circle, exactly what it would be if you did take an end mill and run that part into there. Otherwise, besides using the swept feature, this would be extremely difficult to create that exact shape.
It can be very hand when you're working with machine parts to get an accurate representation of what's going to happen when the end mill cuts into a part or you have different features you're going to be working with. The Swept Cut command can be very useful. It's great for creating special features. The concept is the same as with creating Sweeps. We need to create a profile and a path. The two sketches cannot be on the same plane, and they need to have an orientation that allows the shape to be built.
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