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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.
When using the Hole Wizard, we can use layout sketches from within the Hole Wizard interface. Or we can use predefined sketches to place the holes. We can also use the Hole wizard in a 3D environment that plays holes on multiple faces from multiple angles. To get started, let's go ahead and take a look at the first method. I'm going to choose the top face, and then I'll click on Hole wizard. In this case here, I'm going to come on down to the type of hole. Which is going to be a counter board hole. And then I'm going to come down to ANSI inch, and I'm going to use a socket head cap screw, and I'm going to choose a three eighths hole, normal fit.
And my condition is Up to Next. And I'm not going to add any other things here, just going to go over to Positions. Now, anywhere I place a point is going to automatically add that hole. But before I start placing a bunch of holes, I'd like to actually create a layout sketch to define where those are going to be. So what I'm going to do is I'm going to hit Esc to turn that hole point off. And then I'm going to click on the top face, and click the space bar so I'm looking straight down on it. Now you can see I have some other underlying sketches here, which I'm not going to be using here. We're going to be using those in the next example. But this case here, I'm going to do almost exactly the same thing.
I'm going to start with a center point rectangle. I'm going to start right at the origin. I'm going to drag it out. I'm going to define this with a couple dimensions. I'm going to type in 7.0, and over here I"m going to define this as 16. And then because I don't want to actually have any real lines, I just want construction geometry. I'm going to click on each one of these regular lines here, hold on Ctrl, select all four, and then come over here and click on Make For Construction. Click OK, and now those are all construction geometry. Now what I can do is, I can take this point I made here and I can drag it over and snap it right to that corner.
Now I need three more, so I go back to the point command, and place them on that face. Keep in mind, SolidWorks for some reason doesn't want you to place the points directly over these corners here, so place it next to it first. One, two, three then turn the point command off. And then what you can do is drag these points over to these corners. Looks good. Notice, also in the center it automatically put a hole because of the way that the center point rectangle was drawn. It actually has a point right in the middle. So if you don't want that point, we have to go ahead and delete it. That acutally causes an issue.
And now my whole sketch is acutally undefined in blue. If you click on it, you notice we can drag it around. That's a, a bit of an issue. But don't worry, click back on that origin, hold on Ctrl, and click on Make Midpoint, and it brings it right back. When you're happy with what you have, go ahead and click on OK, and the poles are placed on your part. The next method would be to go back to the Hole Wizard. This time I'm going to choose a counter sunk screw. And I'm going to choose 82 degrees. And for the size of that, I'm going to choose a three quarter inch, so a big one. And I'm going to add a little bit of a head clearance, just a little bit more, 30,000ths.
And then come over here to positions. And notice I have this 3D Sketch, but I don't want to use that one quite yet. I just want to choose the top face. But what I do want to do is, I want to come over here, and notice I have this other sketch that I predefined. What I can do is I can just snap to those corners to quickly place those holes. In the design. When you're happy with it, click OK. And there they are. That sketch was defined on the top surface. And I just predefined it here. In here where the two sketches. So sketch three is the one that was used there. And now is, I just use a basic sketch and it's undefined at this point in time.
So I could drag this around if I wanted to. And I can add some dimensions. But it's not necessary to actually dry those holes. In fact, you can add the holes, and then move them around later and add some dimensions to fully define the sketch. When you're happy, go ahead and exit out of the sketch and notice those holes automatically track and move to the corner points of that sketch. The final method here is going to be a 3D sketch and what I want to do is I want to place holes around the perimeter of this shape. So I want to have a hole here, here, here, all the way around the rest of the part. To do so, lets go back to the Hole wizard.
I'm going to choose a Tap tool, in this case here, it's going to be a 3A16, and my Up to Next condition is not really what I want here. I want a blind hole, and I'm going to type in, I want it to go .75 deep, and I want it to be a half-inch of threads. As soon as I choose that, I'm going to go over here to positions. And notice I have the option to turn on a 3D sketch. Let's go ahead and do that. And now anywhere I'm going to be clicking, it's going to place a point. So I'm going to start again, not on the point itself, but right next to it, I'm going to start placing these holes.
And notice it gives me a preview of what's going to happen. Again, place, place, place. Spin it around. And just place them close to the points where you want to be. There, there and there. So that's allows me to place holes on multiple faces from multiple angels. When you are done with that. Go ahead and click the point command off and what we want to do is drag and drop these little points on to those in points. And notice it alligns tangent to whatever it happens to be on. So this actually saves quite a bit of work, especially if you do a layout sketch first.
Instead of having to make multiple faces, multiple instances of that same Hole wizard. I can do it all at one shot, with a 3D sketch. Click OK. There's all those holes and I can easily modify those later on by just changing one option in the Hole wizard versus having to change multiple sketches on multiple faces. To give you an example of that, let's go back to that hole Instead of a tapped hole let's change it to a regular hole. And come down here. I can choose drill sizes, fractional, tapped drills your choice, any of these. I am going to use a fractional drill size and I am going to choose the what size of hole I would like to type in there.
I am going to choose three quarter inch hole, my blind condition is one inch. Positions stay the same, click OK, and they quickly update. By using a separate sketch to drive the Hole Wizard, we can have a dynamic feature that will adapt to the driving sketch. We can also have the ability to create holes on multiple faces all within one feature.
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