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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.
Creating a revolved cut is exactly the same as creating a basic revolve. However this time, we need something to cut, and the features act a little bit differently. This command also builds on plane creation and sketching skills, so make sure you're up to speed if you're working with complex cuts. In this case here, what I have is a extruded Hexagon and I've got a sketch, Sketch2 here laid out already. Let's go ahead and open that up and take a look. So one of the requirements for a revolved cut is an enclosed boundary. Notice I have a sketched layout here with just the line tools.
So I have a line tool going here all the way around this outside perimeter and goes back and closes itself off. So just to give you an example, let's go ahead and just try out some of these sketching skills. Let's go up here to the line command. I'm going to start right on this upper corner and draw a line over here, draw a line back over here, down to here. I'm just kind of snapping to those corners, down and back over, and then I'm going to drive it all the way back up and close that sketch. So I have one enclosed boundary, all just using the simple line tool. Now what I want to do is add a few of the relationships.
Notice there's a few relationships already added like this on here, perpendicular, so I can define one of those angles, and the other one will automatically update. To do that, let's go up to Sketch Dimension. Come over here and click on this first line, click on this second line. And type in the dimension which is already at 45 which is great, click OK, and then I want to define this length here. So if I hit escape to get out of the dimensioning tool, I can see I can drag this up and down, move it around, and what I want to do is add a dimension. So in this case, I'm using what is called a double dimension.
So I can dimension from this line to the center line of the part. And notice as soon as I put the value in, it gives me a radius value from that line to the center line of the part. And notice as soon as I move past that center line it actually doubles, then turns into a diameter value versus a radius value. So sometimes that's really if you're working with diameters and not radius' to be able to type in the full diameter versus the radius. So it's really dependent upon whether you're on the left hand side, or the right hand side of that center line. I like to kind of use these double dimension values because it makes it easy to type in the values as their full diameters.
Go ahead and click OK, and let's type in 2.2 for instance. These are obviously not the right values. I'm just giving an example of the size. The correct values are right up here. Now, a couple of other things we might want to add. Maybe another dimension here between these 2. So click on the first one. Over here to the second one, and type in the value. And notice as I put these values around, it changes. So inside of here, I've got this 52. If I move out here, it changes the way the value is inputted. Same thing over here. Same thing over here. So make sure you're placing the value where you'd like.
For instance right here, it may be 45. And then once you have the value placed, you can always move it out. And out of the way differently, as long as you're placing it correctly the first time. Once everything looks good, we can probably add a few other dimensions, but I'll skip that for right now. I'm going to go ahead and actually just delete these values and sketches, so we're ready to actually revolve the original sketch that I had. Let's go back to Features, let's go to Revolved Cut Choose our axis of rotation which is going to be that center line, and by default it's using a blind rotation of 360 degrees.
Go ahead and click on OK, and you can see what happens. It just trims out that material off the part. Now let's go back and take a look. Go back to Revolve Cut 1. Click on Edit Feature. And you can see that I've got a couple of other options here I can play with. So instead of Blind, I could use maybe Up to Vertex. In that case here, it's taking this sketch, and it's going to revolve it around till it sees a certain point. And if I choose a point like this one, notice it revolves around and cuts up to that point. Pretty handy. Click OK. You can see what happens. And go back again.
Modify that feature again. This time I'm going to come down to up to surface. The problem with up to surface is that it needs a surface to completely end that feature. In this case, we don't have one of those surfaces, so it's not going to work. But if you did have a surface that was extending maybe from the center line of the part out to one of these points, you could use that to end that revolve. Offset from surface, exactly the same thing if you had a surface you could offset from it. But its not really going to work on this example, but I did want to point it out. And finally mid-plane. Mid-plane allows you to go both directions with whatever angle that you want so in this case here maybe I'll type in 90 degrees.
And you can see that it's going 45 this way and 45 this way to make a 90 degree cut. And I can click the up arrows or down arrows to continue that on, and it goes both directions with that cut. So, pretty handy. When you're done, click OK. And you can see what we have. Again, go back to the feature. And I'm going to go back to the original blind cut. At 360 degrees. And notice down here, we have this thing called selective contours. Selective contours allows us to choose multiple items to revolve. In this case here, I only have one enclosed boundary, so it's really not going to make that active.
So I want to go back and actually show how that works. So click OK, and let's go back and delete that feature altogether. So click on Cut Revolve 1. Press delete on your keyboard to delete the feature, click Yes. Notice if I delete the feature, the sketch is still there. So this time I'm going to go back to that sketch, edit the sketch, and I'm going to add a few other items to the sketch. Number 1, I'm just going to add a rectangle directly below this. And I'm going to not add any dimensions right now cause I'm just going to use this as an example. Now, go up to Features, jump up to Revolved Cut, and choose my axis for rotation, which is this.
And by default, notice it revolves both of those shapes. Click OK. And there's an example of how it's going to look. But if I go back to Revolved Cut, I can actually go down to Selected Contours and I can choose Maybe just one of these contours that I want to revolve. So even though I have 2 shapes in that sketch, I can only choose to revolve maybe just one of them. Or go back to the feature again, this time here I'm going to choose the second one, and I'm going to get rid of that first one by hitting Delete on my keyboard, and click OK. And you can see it only does one of those cuts, or you have the option to go back and choose both of them.
So go back into this box Choose this other contour, click OK, and you can remove both of those shapes with one Revolve Cut. Revolve features can do a lot with only very simple input. The basics are, choose or build a sketch, choose an axis of rotation, and then select the degrees of rotation and just simply click OK.
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