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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.
Mirroring is the best way to double or quadruple your efficiency. Look for part symmetry. If the right and left sides look the same, then mirror the part. Save yourself some time and make better parts. Here's an example. Take a look at this part here, we've got a simple sketch, sketch one, with a basic strewed. Let's take a look at the sketch, you can see that, if I click on normal to, I've got a lot of dimensions here. I've got holes in the corners. I've got dimension on each one of these. There's a lot of time for efficiency here. So I could delete a lot of this stuff.
I could say, these holes are all equal. I could delete these here and make them a between these two, so we could refine this a lot more, but a lot of times you'll see this type of extra work being done in a part design. It's a lot of extra stuff. You're doing the same work over and over again. You're drawing four holes when you really only need to draw one. You're drawing all these other lines and dimensions when you really only need a quarter of them. Cancel out of this one. Exit out. Let's go take a look at how to do this correctly. Window, let's take a look at this other file that I have open which is 9.4-2, and you can see that's actually just one quarter of that same part.
Same Boss Extrude. Take a look at the sketch this time. You can see we have far less dimensions. I got a dimension of five inches across, four inches tall, and defining the hole is three quarters of an inch, and it's one inch from the corner. And I have a couple lines down here that is the same length, defining that distance from the edge. Exit out of that. You could see I did an extrude of that part and I have one quarter of it. Come up here to Features, come over here to Mirror. Face or plane to mirror about. We're going to pick one of these edges, either this one here, or that one there, it doesn't really matter.
Pick that first edge. Now we can come down here to Features to Mirror, and that's what everybody wants to do. Skip that one, though, close it up, hide that one, come down here to Bodies to Mirror. This is really important, you're going to make this error, I guarantee it. Go to Bodies to Mirror. The software always defaults to Features to Mirror, but in a case like this, I don't want just one feature, I want this entire body. Come down to Bodies to Mirror. And click on the entire body. I want to bring everything over at once. Click OK and there it is. That simple. Again, come back up to Mirror again, this time, face your plane and mirror about.
I want to this entire face here. So click anywhere on that face, and then come down again. Bodies to mirror, not features to mirror, but bodies to mirror. Click on the body. Click OK. And just that quickly, we've made it a very robust part that's easy to update and easy to work with. Now any changes I make to that original feature. Notice there is a boss extrude one, plus two mirrors. Go back to this boss extrude one, anthing I want to change here. For instance, if I go to sketch one, open the sketch or edit sketch. For instance let's go ahead and add just a little rectangle.
Here he is. We could dimension if we wanted to but, in this case, I'm just going to provide an example. Exit out. Guess what happens. Automatically, that rectangle propagates across both of those mirrors because it's part of that original body that we mirrored. If, for instance, if we only wanted just a hole on one side, and not the other one, that's when we use features to mirror. Let's take an example. Click on the top of this thing here. Click on Sketch. Start a sketch. Make a hole. I'm just going to drag a hole out here. And we'll do an extruded cut. And we'll extrude it 0.1. Now that is only on the right hand side of this part.
I want it over here on the left hand side of the part now. What do I do? Okay, first, going to come up to Mirror. It's going to ask me what's my face or plane to mirror about. There used to be that face here on the edge of the part because I had only one corner of it drawn. Now I don't. So take a look, maybe you have a plane like the front plane or the top plane. In this case it happens to be the right plane. Choose that plane and then instead of bodies to mirror, because I don't want to bring the entire body now. I only want this one feature. So in that case, go down here to Feature, pick that one feature, click OK, and you can see that just drags that one feature and mirrors it over onto the other side of the part.
So there's both body mirrors and there's feature mirrors, both of them are extremely powerful and easy to use. Just make sure you're choosing the correct one for the task you're looking to do. Mirroring is a great time saver and makes modifying and updating parts quick and efficient.
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