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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.
Reuse of sketches is one of the best ways to save time and be more efficient in SolidWorks. Creating blocks is as easy as selecting the elements and choosing Make Block. Then we can use that block in other sketches. Imagine the situation when we have a very complicated sketch that makes the cutouts for a motherboard. You can see here we've go a lot of entities and a lot of sketch dimensions in this. To create this. I don't want to go ahead and create this over and over again, every time I might want to use that same motherboard in a new product, so why not take all these entities of the sketch, and turn it into one big block? To do so, let's go ahead and select all of these, come over here to the Blocks toolbar, and click on Make Block.
That grabs all that, puts it into one big block that you can see over here. Here are all the entities that have been added to the block. You can even come down here and choose an insertion point. That'll put a little blue arrow on the screen, and I can place that wherever I want. Well I'm going to drag that right down here were the origin is, and so if I put in a new design I'll be using that same exact point. When you are happy with that go ahead and click OK or the green check mark. And now you still have the same sketch but all those dimensions have been hidden, all those relationships have been hidden, and now you have one easy to manipulate block that I can then save out or reuse in the same sketch.
So in this case here, I actually want to take this somewhere else. I want to go use it in a different part. So what I'd like to do is actually save it out to the file system. To do so, come over to where it says Block 1, right click on it, and click on Save Block. I'm going to go ahead and go up to the desktop, come down here to Exercise Files. And inside of chapter ten, I'm just going to go ahead and inside of blocks, I'm just going to call this block one, and it's totally fine. Go ahead and click Save, and now we've saved that block out to the file system. Now, if you didn't want to keep this as a block in your existing file system here, that's okay, we can actually use the Undo command, and turn that right back off, and turn it right back into a regular sketch, now that we've created a block.
Your choice. Once you're happy with it, click OK, and then close out of that sketch. And now I'm going to go over to another sketch on a different part. So I'm going to go to Window >Tile Horizontal. I'm going to take a look at this other part. Here's the part I actually want to put that cutout into. So I'm going to go ahead and choose the top face, click on Sketch, then I'm going to come up here to Insert Block. If you don't have this toolbar shown, you can always turn it on by right-clicking anywhere in the area up here, and make sure you have blocks turned on. Or you can get the same exact tools under Tools, come down here to Blocks, and Make or Insert Block.
In this case here, I want to come up to Insert Block. I'm going to go ahead and find that block that I just saved out, which we saved on the desktop. Under, exercise files, chapter ten, Blocks and we called it Block1. Go ahead and click on Open and notice that block is now attached to my tooltip and I can place it anywhere I want. In this case here, I'm going to place it right in the middle and notice, as soon as I do, it stays active and it stays on my tooltip and if I don't want to place any more of these, go ahead and hit Esc to turn it off.
Then I could add a couple of dimensions, maybe from this edge here at the beginning of that first hole, 1.5. And from the bottom to that first hole, again maybe 1.0. Notice as I dimension one of these, all the other items move because they're evaluated as one combined unit. Now, I can either extrude it, I can cut it. I can do anything else with that sketch geometry. In this case here, I'm going to go up to features and I'm going to go ahead and do an extrude cut to cut those holes through the part. I'm going to click on Up to Next.
And click on OK. So I quickly added these cutout holes to an existing part, very quickly. Just by reusing that same geometry and creating a block. From those sketch entities without having to redraw everything and reattach all those dangly dimensions to this part. Additionally, if you're working with imported data like AutoCAD files. Or exporting files from graphics programs like Adobe Illustrator. Blocks can make it really easy to get those files into SolidWorks and easy to work with.
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