Designing the base component - Fusion 360 Tutorial

- [Instructor] So let's get started here, by creating the base part for my robotic arm. So let's start by just creating my first new sketch. And I'm going to sketch on my top plane here. I'm going to use a center rectangle, and start the center of my rectangle at the origin point there. And I'm just going to throw in some dimensions, I'm going to use maybe 180 millimeters by 180. And notice I'm using millimeters here, but of course, you could use inches if you'd like. And again, I'm just kind of making up these dimensions. So of course, you could use whatever dimensions you might like. Once I'm happy with that, I can finish off my sketch. And if it's looking good to me, let's extrude this up. Maybe let's say 10 millimeters, I'm happy with that say, OK. Next, I want to add another sketch. In this case, instead of using one of my existing planes, I'm going to sketch on the top surface here, so I'll click on that top planar face, sketch a circle at the origin point and maybe throw in a dimension of 140 millimeters. If I'm happy with that sketch, finish off the sketch, and extrude, this, maybe 100 millimeters, let's say, if that's looking Okay, finish it off. And I'm going to create one more new sketch here. In this case, I'm going to use the front plane here. And here again, I'll create another center rectangle, and I'm going to throw it somewhere in the middle here, say about here. And again, I'll just make up some dimensions. Let's see maybe 40 millimeters by 80 millimeters, something like that. And then I also want to position this rectangle, so I'm going to throw in a dimension maybe from the center point of the rectangle, to my origin point, and I'll give that a dimension of, let's say 60. Looks like this sketch is now coming in, fully dimensioned, fully defined, so that looks good. If I'm happy with that, I can finish off this sketch. And again, I'll extrude this new sketch, maybe, let's say 100 millimeters. And notice it looks like by default, this is coming in as a extruded cut, when in fact, I actually want an extrude. So I just want to check out my options here and notice the operation is by default jumped into a cut. So I want to change that to a join. That's looking a little bit better to me, so I can hit OK to finish it off. Finally, I'm going to create one more sketch. I'm going to sketch on this top surface here. And let's say I want to do a circular cutout here, I could just sketch out another circle, or I could make use of the offset tool. So I'm going to go to my modify tools and find Offset. And I want to offset from this circular edge here. And let's say I want to offset this maybe five millimeters. Notice it looks like the offsets coming in on the wrong side right here. So I can just type in negative five, or if I just hit flip, soon it automatically jumped to negative five. And now that's the offset direction that I want it. If I'm happy with that, I can hit OK. And that's looking good, I can finish off my sketch. And finally, one more extrude and I want to cut away this portion here. Let's say I want to go down maybe three millimeters. So I'm going to type in a value of negative three here. It looks like this is cutting instead of extruding, but I can always double check, just by taking a look at the operation and notice this is a cut as I would have wanted, so I can hit OK to finish it off. And here we can see we've created the general shape for the base of my robotic arm.