In this lesson, we'll go over detailing a top down view sketch. After completing this lesson, you'll be able to create a sketch mirror and create a sketch offset. Since we hopped out of the top down sketch, let's go ahead and let's just rename it. I'm going to call it top down shape. And again, you don't have to follow exactly along with what I'm doing, my naming conventions, or even naming the sketches if you really don't want to. This is the design process that helps me as I'm going through, and this is really because, once you get a dozen or more sketches, which we're going to have quite a few more than that, it makes it a lot easier for you to come back to the browser and figure out what each sketch was. Sometimes you might decide to do the Keep Out sketches first, sometimes they might be fifth in line, you might have some geometry first and so on. When we look down here at the bottom, also when you hover over the sketches in the timeline, you can see exactly which component it belongs to, and exactly what the name of that is. So, we're going to double click on the top down shape. We're going to edit, and we're going to start to add some mirrors. So, under the sketch drop down, we want to go down to mirror, and the objects that we want to select are going to be the solid lines as well as this 30. And we're going to mirror about this horizontal line. If we zoom out a little bit, go ahead and say OK. So now what we've done is we've created half of the design. Now remember, we're only drawing half of it and we're going to mirror it to the other side. It really helps out with symmetry, because you know with 100 percent certainty, that everything on the right side is going to be the same as everything on the left side. At least until there's some unique feature that has to crossover. We're also going to take this vertical line and we're going to change it from construction, we are going to change it back to a normal geometry. So now we have everything on the right hand side that we need to start creating the shape. At this point in time, I'm going to go ahead and stop the sketch, and notice that, this line extended past, because it wasn't part of that symmetry, it wasn't part of that mirror. Sometimes it's hard to see when you're in the sketch. So, sometimes it can be helpful to exit the sketch, and then you can come back and you can drag it into place and have it snap to that geometry. Now when we stop the sketch, it makes a little bit more sense. There are a lot more elements that we need to add in. But at this point in time, I'm going to break them out into different sketches. Now the reason I like to do that is because, when I go back to make edits or when I go back to make changes, sometimes it can get overwhelming to see dozens and dozens of constraints and dimensions and all those things. So, it really helps me to come back after the fact in a separate sketch and just project geometry as needed. So let's start a new sketch. Again on the top plane, we're going to select x, z. And now what we want to do is we want to start to create some of the offsets. Because obviously, we're not going to make this just one big solid body. We're trying to keep the structure as minimal as possible to keep it light, but also keep it as strong as possible. And I know that's a little bit tough to do, so we're going to take a look at how we can achieve this. So with this profile, we have a few things going. We have a complete closed profile here, and we have a complete closed profile here, as well. We also have some reference lines, for where some structure is going to be. And we potentially have sort of a layout of where we need openings, or where we want to minimize the restrictions to let as much air flow through as possible. So let's start by taking this outside profile and we're going to offset it 10 millimeters. So I'm going to go around, and rather than use the whole profile, I'm going to grab what I want, and I'm going to use my marking menu, and we're going to offset this 10 millimeters. I'm going to type in 10, and I'm going to say OK. Now, I noticed that I didn't chain the selection, and if I come back and I turn off the top down shape, notice that, I don't actually see anything here. So I'm in this new sketch, but my offset is actually not in this sketch. So, if we go back to the top down shape, notice that the offset is actually in this sketch here. So this is something that we need to be aware of. So I'm going to undo, back before that offset. And we're going to look at how we can bring this information into the current sketch. So in order to do this, we're currently editing sketch five. Under our sketch dropdown, we have Project/Include and Project, which is the letter P. So this will allow me to bring in information that I want to have in this sketch. I'm going to go ahead and bring the center line in as well. And I want to bring this line in as well, and say OK. I'm also going to go ahead and draw circles, here as well as here. I'm going to make both of these equal to each other, and then I want to give them a dimension. I don't want them to be exactly what the prop is. I actually want them to be just a little bit bigger. So I'm going to give it a dimension between these of two millimeters. Now the reason I did this is because, this line is going to be where a support is going to be located. So, I don't want it to be exactly five, I want it to be a little bit bigger so I have enough room. And this isn't going to be directly in contact with the propeller but it's going to be above it, so that way I know that I'm not obstructing the air flow, or at least as minimally as possible while still giving it structure. So now if we hide the top down shape, notice that we have the offset and anything that we projected, for instance, I added a dimension from here to here and automatically projected that into my sketch. So now what we're dealing with is a complete copy of some of the shapes in the top down with the exception of not looking directly at some of the construction geometry that we had. So this helps clean up a bit what we're looking at and helps make our offsets more realistic. So again, I'm going to use my marking menu for offset, and if you select Chain Selection, it will only carry as long as there's tangency. But what you want to do, is you want to select all the entities that you want to offset, and I'm going to bring these in 10 millimeters and say OK. I'm also going to place a circle at the center here. That's 28 millimeters. And I'll do the same thing over here, and I'll make these equal. Now the reason I didn't project this specific circle is because I don't necessarily want to drive it off the 28 that's in the first sketch. I might want to make it bigger or smaller. This is going to be the mounting circle for a motor, which has a 19 millimeter diameter bolt circle. And all this information is directly from the DYS manufacturer's website, or you can find it on various websites. Wherever you find the motor for sale, generally, that information will be located there. Now there are a few more things that we want to add in here. I'm going to start by sketching a line from the center of the motor to the origin and back up to this one. So this is going to be the location of a support. It's going to allow me to add some structure to where the motor is supported, and of course, the motor actually needs to be supported by these walls as well. We also want to add a bit more. We're going to go from here down to here, and we're going to eventually add some structure inside of this center as well. So for right now as we look at this, we've got the motor floating out in space, we've got these 10 millimeter thick walls on the outside, and we need to start adding again some additional thickness. So I'm going to take these lines and this line and I want to offset those as well. So again using offset, I'm going to grab both of those lines and I'm going to offset them five millimeters, and we're going to go minus five. And we're going to repeat it again using the marking menu, and this time I'm going to offset them positive five, and keep in mind this extends out but I don't need to use this. The selection process inside fusion when we go to do things like extrudes it's very simple, so I don't need to worry about trimming this geometry. And oftentimes, if you go to trim geometry, what'll happen is it's going to undo some of those dimensions and constraints. So oftentimes, it's better to just leave it in there. Now one thing I also like to do is I'm going to take this number here and I'm just going to click on this one and say OK, so that way the offset is controlled completely by this one here. So if I change this offset to six, it'll change the other one as well. So, a very easy way for us to make sure that we keep those dimensions in check. We can also do that with this 10 millimeter and just say that this five is half of the 10, if you want. So, there are various ways that we can do this. Now again, we've got some progress. As you're learning fusion or as you're starting to get into this, it's a good idea if your sketches are going to be very detailed, if you're going to have to add a lot of information, to go ahead and stop the sketch and save the file. So that way you always have a point that you can come back to. Let's say that you get pretty deep into this sketch and you decide that you don't like it, and you want to start to undo it. Well, if you have exited the sketch and saved it, then you have a version of the file, in this case, version four, that has that sketch. And if you save a later version with the more complicated sketch, you can always go back to that version as well. So it's pretty flexible and I encourage you to save often, so that way you have various versions that you can reference if needed.