Create and extrude your aesthetic curves - Fusion 360 Tutorial

- [Instructor] I've loaded up the 6-10 Example File, so we have a headphone hanger, but it doesn't look quite like the original drawing. If we bring back the Canvases here, and have the mount industrial design, yeah, we do have a band up here, and we do have little baseplates that somewhat match the design, but we didn't do any of this, so that's what we're going to do. I'm going to create a sketch, but before I do so, notice that my original design did have these arcs in the center of this mount. But this mount is no longer symmetric. We did do a Symmetric extrusion to here, but then we added on five millimeters for the baseplate. So, how to put these arcs in the center? Well, just that, we would create a center point, or what's called a midplane. Under CONSTRUCT, select Midplane. So, it's in the drop-down menu here. And what Midplane does is it creates a plane between two objects. In this case, we want to click on the front face and the back face. And now, you can see that this new plane that's created is directly in the center of those two, no matter where these change, if you happen to change your design later on, this will always be in the middle. And then, CREATE a Sketch on this midplane. Great. If we bring back the Mount ID canvas, we can see that I wanted to create some arcs, so let's do so. And again, these do not need to be entirely accurate, but we want to create an arc, and we want to snap that arc to the existing shape. But notice we don't get the snapping function that we did in previous sketches. That's because we did not create our sketch plane on the actual object, it intersects the object, but there's nothing here to intersect. So, here's a couple ways to get that to work. Click on Slice in your SKETCH PALETTE right here, and this is more of a visual thing. This says, okay, I've now sliced all bodies based on where they intersect, but again, you are not able to snap your command to this. So, we need to fix that. Go to CREATE, Project/Include, Intersect. So, we're not going to project the body, but we want to find where this body intersects with our sketch plane. And I'm going to click on Bodies because I want to have the projection be everywhere where this body intersects. And if we click on this body, and we click OK, we can actually turn off the visibility of this body, and now we have this projection. So, these are kind of this magenta, purple color, which means that this is a projection. I'm not able to edit these. This is literally where that body intersects. So, now when we CREATE our 3-Point Arc, we will get the snapping function. You can see that it's snapping. And you notice that we do not have the ability to see the mount anymore, because Slice is turned on. Slicing does slice through everything, and if this attached canvas is in front of the slice plane, which it was, you're not able to see it. So, you want to turn Slice off, and then you'll be able to see your plane. And if you ever scroll around and you get kind of lost, you can always click Look At on the SKETCH PALETTE to be brought back. And in this case, we're looking at it from the back. You can rotate around, and now when you click on Look At, it will orient you in the proper way. So, go to CREATE, Arc, 3-Point Arc. And again, this is not going to be super accurate, but also when you click over here, your arc is not going to be centered. That is totally okay, we'll fix that later. But what you do want to do is you do want your arc to be centered on this center line. You can kind of see that my mouse is snapping to the center. We do want that to be there, that is fine. That's nice. So, now click a Line, click on Line, and connect these two edges like that. Now, apply a Horizontal/Vertical constraint, so click up here, and then click on this line. What that does is this line is now absolutely horizontal, but because it is coincident with these points, these points are now going to be on the exact same line as each other, so your arc is going to be accurate. Press Escape to exit that tool. You don't really need this, this is a helper line, you can press the X key on that line to make it more of a Construction line, and not create a profile. We can use the O key, O for OFFSET, and you see when I click that, it wants to offset everything. I don't want that. If I press the O key and turn off Chain Selection, and click on this, I'm just getting this line. And I'm going to bring this down probably negative five like that. Because I had the X key turned on, this actually came in as a Construction line, so I'm going to select that and press the X key to bring that back. And now, notice that this is a closed profile, if we really, really zoom in this offset does not perfectly match up with this profile. That's totally okay. This is still creating a closed profile. You could use the MODIFY Trim command to trim that off, but then you would remove the Offset constraint, so that is totally okay to keep right there. That looks kind of nice. Now, go back and say CREATE, Arc, 3-Point Arc. I'm going to create an arc, you know, somewhere on the bottom, and somewhere matching my image up here, like that. And again, if you can't really see this you can turn off the Canvases, and that makes it a little bit easier to see. I'm going to hit the O key for OFFSET again, and offset this. And I'm going to offset it probably to about six millimeters, and I'll show you why. We're totally fine up here, but it does not match down here, so how do we get this arc to extend down there? Well, easy. Go to MODIFY, to Extend. When you have this tool and you hover your mouse over, you will see a little extension. So this is snapping to something else in the model, I think it's probably this line, but if you click once, extends, it still isn't there, hover your mouse over, click again, now it does extend. That's pretty nice. Press the L key for Line. What we're going to do is just create a Mirror line in the center like we did before. So just any sort of line right in the center and do the Mirror command. So go to CREATE, to Mirror. Click those two objects, and then the Mirror line over here, and click OK. Now notice that we have all sorts of lines that are going over other lines. They're all creating closed profiles. That could be totally okay, you would just need to remember to extrude all of these profiles later, or you could use the Trim command to really trim these up, but then all of these other constraints may change or be deleted. In this case, we'll just keep them. So, if your design looks something like this, click FINISH SKETCH. We're going to bring the body back now. All right, now that we're out, click on this bottom arc, this arc, this arc, and any other shapes on the middle, right-click, and go to Extrude. Because we're on the midplane, we want to, again, go to a Symmetric extrusion, and just bring this out. If we want this to be really, really strong, we can bring it out. So, what I'm going to do is bring this out to about 17 millimeters, and we're at Join, and click OK. This has done nothing. It made it a lot more structurally sound, but again, for our headphones, we don't really care, it's not going to be a very high stress use case, but it is a lot more pretty than it was before.