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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.
Effective use of construction lines in Construction Geometry is the key to being an efficient and effective designer. Many times, sketches can be fully defined without even a single dimension. By tying your sketch entries into existing geometry, we can build powerful sketches that are dynamic. Let's consider the case of 2 holes that need to be equally distant from the center line of a part. Let's take a look at what to do. So in this case here, I can go in and take a look at the feature itself, and below that is the sketch. Let's go ahead and edit that sketch and take a look. Okay, what we have here is a under-defined sketch.
And I want to place a hole about here and a hole about there. So I could Start off with a hole, I could place the hole here, and maybe come over here and place another hole. And then what I could do is maybe add a dimension here and tie it into the side, maybe we'll say one inch there. And we do the same thing over here, again one inch. And of course, we want to do the same thing over here again. Click from here to here. Okay, one inch, and then of course, we could dimension these things one inch there, and maybe one inch there. So what happens here is if I move the outside sketch here, those follow along.
That's okay. Move it over here. You know, they are equally distant from the center line and everything looks okay, except, you know we're adding a lot of the same dimension over and over again. And it doesn't really look that great. And what if we really wanted this hole to be in the center between this line and this line? Then, it makes it a little more complicated. So let's look at how to do this correctly the first time. So what I'm going to do, is I'm going to go ahead and just delete all that. You can delete all those dimensions as well. And we'll start with a little bit better methodology. First off, I'll start with the center line. So from the center point of this or from the origin, I can choose a line from here.
In fact I can make actually 2 lines, containing the second line all the way up to the top. Now I've got 2 lines here and you can see I have a point between the 2. And I say hey this line here, hold on Ctrl. Select this line here and say well let's make these equal. Then what I can do is make another line here. Just bring it across here. And I could make that point this point here, and that line, hold down control, make a midpoint. Now I've got a line that's midpoint in the center there, so if I move things up and down, it's all moving parametrically. I'm doing all this before I've even added the holes. Now I can grab a hole, or a circle.
Drag the circles out. Might as well make them equal. And now you have a much more robust design. Now all you need to do is add maybe one dimension from here to here. We just type in the same one inch dimension and it controls both sides and anything I move in the design will automatically update. If I move things around here, it'll automatically update as well. Makes it a more parametric design that's linked to other items. In fact if I wanted to, I could delete this altogether. Maybe what you'd like to have is this hole in the middle of. This little tab. In this case here, I can say well, why don't I snap to the midpoint, and snap to the midpoint of the hole, and then make this line here vertical.
Now when I drag this out, it's automatically always in the middle of that tab. I drag it up again, always in the middle of the tab. So very robust design, and you can see, you don't even have one dimension here. Locating where these holes are. The only dimension you might want to add is the size of the hole. Make it one inch. Add a few other dimensions to the size of the actual part, but we had to have to put that in anyways. When you're happy with what you have, save out the sketch, and you've got a more dynamic, robust part, using construction geometry and center lines.
Building good construction geometry is the single best way to make better sketches, and to leverage the power of the parametric capabilities of SolidWorks. Always try to think through how your sketch will behave and try to minimize the excess dimensions.
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