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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.
Now it's time to take that to the next level by linking in the location of the holes, to another part. In order to do this, first we need to edit the part from within the assembly. Then we simply open the hole wizard and choose a reference point in another part. First off I want to point out that I have these two parts mated together so they're sliding, but they're not, fully located. So this part can slide around on this bottom plate. And what I want to do is I want to create some tapped holes. In this plate here, so this piece of hardware here can bolt these two together. This is a half 13 socket head cap screw, and I already have those corresponding holes in this top plate here.
And I just want to go ahead and make the tapped hole again at the bottom plate. So first things first, let's click on this part here, and instead of opening the part, I want to come to the next little icon over and say Edit Part. And notice everything turns transparent. And you can see over here that this part is blue, showing that it is being edited within the assembly. If you open that part up, you can see that it's just basically a boss extrude. So, pretty straightforward. Let's go ahead and click on the top surface. Come up here to, under the Features tab, to Hole Wizard, and go ahead and choose the Tapped hole.
We're using ANSI inch, it's going to be a tapped hole. And for the size, I want to make sure I'm choosing a corresponding size to the piece of hardware we're using, which is going to be this half 13. And for my condition, I don't want to go blind. I actually want to go up to next. Same thing with the threads. It's a through hole. And I want to show it with a cosmetic thread. And everything is pretty good, so let's go jump over here to positions. And notice the Point command turns on alright, that's the basic for the hole wizard, wherever you put a point it's going to put a hole. So I can put a point out here, it's going to put a hole.
I can put a point over here, it's going to put a hole. Or, if I click on space bar I can snap to the, notice how if I go over these outside edges of these existing holes, it shows me the center point. I can snap to the middle of those holes. Very easily, just go over the outside edge, and snap to that middle of the hole. If you don't see those, just jump over the edge first and it shows you the center point. And again, zoom in, zoom out. Grab those holes. And notice, as soon as I'm done, turn the Point command off or hit Escape on your keyboard. Those holes are fully defined, they're black.
So these points are defined as black, these ones over here I dropped on there first are blue they're still undefined so I can move those around if I wanted to or if you don't want them hit Delete on your keyboard and get rid of those. Get rid of that one as well, and you can see we just have those four holes now on the screen defined directly under the existing holes. Go head and click OK to exit out of the Hole Wizard. And go head and exit out of that part so you're back in the assembly mode. And now you can see directly below these holes here are those tapped holes. Now what happens if I move this plate over to here? Notice at first they don't move, but as soon as I let go I come up here to Rebuild.
They automatically follow along. So very powerful, right. So wherever I move the plate, I'm going to have the corresponding holes directly below those points. And there's no dimensions, right. It's wherever they are. If I come back to this plate here, maybe I edit the part and change where everything is. Take a look at the holes, take a look at the positions. It's just a hole wizard snapped to another point. And if I exit out of that, from my original base sketch here you can see that I've got a couple dimensions here. So if I change the size of this to two inches, part gets smaller, I go back.
Notice the holes automatically change. And when I come back here to the assembly, Rebuild, again, those holes automatically move in to the smaller size of the part. So really powerful. Linking things together, using the Hole Wizard, using in-context modeling is a really powerful way to move parts around, change things, and no matter what your changes are, as long as they're not. Removing that plane or that face or something else that the part was created on, those holes will automatically track, and it's really a quick way to work with the designs that are very robust and can adapt to the changing parts.
Using the hole wizard in context is a great time saver, and using this technique can be a nice little design improvement. To create a mating hole pattern we don't even need the spacing or locations, all that information is received from the attached part. If that part changes the corresponding holes update and life's good. Changes are inevitable and the more self solving features you can build into your model from the beginning the more your model will pay dividends in the end.
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