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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.
There's some special tools and techniques for using the dimension tools with holes and curves. By default, hole dimensions relate to the center of a hole. However, in some conditions, you might want to actually add a dimension to the edge of the hole. I'm going to show you how to do that. So I've got the Dimension Tool turned on right now. And I'm going to zoom in here on this model. And I'm going to dimension to this hole. So by default, if I dimension from this edge here to any one of these outside edges of the hole, it automatically chooses the center point of the hole. And what you can't do if you delete that. If you choose the first baseline dimension and then you hold down shift, it actually allows you to either choose the inside of the hole and place the dimension there.
Or, you can choose a baseline dimension, hold down shift and pick the outside of the hole. And it'll pick the outside of the edge. So this is really handy when sometimes you're using a specialty type of hole. And you don't want to specify exactly the spacing to the center point, but maybe to the edge, or the gap distance between that and the edge to make sure you've got enough clearance. So, it's a great way to use that. By the way, you can also use the same exact technique when you're actually using sketching to draw out holes. Instead of automatically always choosing the center point, you can always then choose one of the edges of the hole. It's a great way to use that tool.
Next thing I want to point out is if you have something like a curve right here, and you wanted to dimension to it. Normally you'd dimension here, and you'd try to like say, well, I'm dimension to this curve here, but that's going to kind of give you this line segment here, and going to the midpoint of that line or to the center point of that arc. That might not be what you want, a lot of times what you want actually dimension is to this virtual sharp that's out here, and you just don't see that virtual sharp. So what you need do is create a virtual sharp, and there's no real tool. You see up here, there's nothing that says, hey, create a virtual sharp. So it's a little bit of a cryptic technique, but what you do is you click on the first line, hold down Ctrl, choose the second line that you actually want to create the virtual sharp between.
And then just go up here and click on the Point command. And as soon as you do that, notice it continues these lines and actually produces a virtual sharp. Now that I have this virtual sharp here, I can use it to dimension. I also want to point out, if you go up here to the Options. If you come over here to Document Properties, now to Virtual Sharps, you can show it how you would like to actually display that sharps. So I can make it a plus, or any of these other styles. Click OK. And then my sharp turn into just a point. And now when I want to dimension. I can dimension from here to that point and again from here to the point over here.
But we don't have, again, a virtual sharp. So let's go back, click on this line here, click on this line here, click on the point. Produces a new virtual sharp, and now you can define the length from this point to that point, along that edge. It's a nice way to add virtual sharps to your designs, and it's great for using sheet metal for machine parts whenever you need to actually dimension to a virtual sharp. And then you can come back and add, for instance, a radius dimension here, showing what that is. You can click on this little point here, or this little dot to bring the dimension at the inside or the outside, depending on how you want to display it, and then click OK.
A couple of really neat ways to work with curves and holes with a few things that are kind of hidden inside of SolidWorks that you might not automatically know about. The commands are the same for working with holes. However, there are a few simple modifiers that are not overly apparent. This movie should give you a good overall view of the tools and techniques.
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