Adding internal features - Fusion 360 Tutorial

- [Instructor] On plastic components, you'll often find the most complex geometry is on the inside. Ribs, webs and bosses can take on many dramatic shapes and remain unseen to the customer. Yet this is the geometry that helps to keep the part in shape and make it possible to put plastic components together. In this exercise file, we already have the sketches needed in place. If we expand the Sketches folder, we'll see that they're all named. Two of them are switched on, but all of them are prepared for you to go through these steps. We'll begin by creating the openings for the screen and the vent using the simple Extrude tool. Selecting the screen profile and the vent profile, we'll extrude this all the way through the body. Making this cut, we'll open it up. Next we want to create the bosses that will be used for the button openings. We'll turn on the button sketch, and either using extrude again, or press pull from the marking menu, we'll select the two profiles, setting the extent to two object and selecting the inside face. This will create the geometry needed to support the buttons. Next, I want to use a tool that's most commonly used for plastic parts in a slightly different way. I'll turn on the screen sketch, as we're going to create a support for the screen to attach to the housing. But rather than offsetting the profile, I'll use the Web tool. Selecting the perimeter of the screen, the Web tool right now is set to symmetric into next. So, it's building 3D geometry out to go flush to the back of this tool. Using the flip direction button, we can see that it starts to build out through the model, and come tangent to the farthest face. If I change the thickness option to one direction, and then transition the thickness to be outside of the opening, we'll see that it no longer goes through the model. We'll set this width to minus two. And that is what we need for our support. We'll click OK to create the geometry, and then we can turn the sketch off. While we're at the Sketches folder, let's turn on the rib sketch. The rib sketch is not a complete sketch. It is just a partial sketch. It doesn't come in contact with either the inside face or the cylindrical face of the boss. But with a rib, that's all you need. So, I'll start the rib tool from Under the Create panel, select the partial sketch, and it will fill in the space, not only following the curvature of the inside of the housing, but the cylindrical face of the boss. Two millimeters is correct for the width. So, we'll create it. Next, let's create a pattern of ribs around that boss. Using under Pattern, circular pattern. We'll set the pattern type to features. And in previous versions of Fusion 360, we used to have to select features from the timeline. But Fusion 360 has been updated, to allow us to select that rib feature directly from the canvas. We'll select the axis, and three is just what we need. We'll click OK, and we'll see that the new ribs are following the contour of the inside of our part as well. Now, let's create a rectangular pattern, using features of both the original rib and the pattern of that rib. We'll set the direction using the inside of our screen support. And we need this to be two instances at 26 millimeters. When I click OK, we'll see that these new ribs also follow their own contours to make sure that they fit the inside of this model. To complete the boss, let's add a couple of holes to go through each boss. If we remember the sketch for the buttons, had a center line that ran from center point to center point. Using the Hole tool, I can select those center points to place holes all the way through the model, with a 13 millimeter diameter, placing both of them at the same time because they're based on sketch points. Finally, let's turn on the grill sketch. The grill sketch is built on a work plane that sets inside the opening of this vent. For this feature, we'll use the Web tool again. Starting the Web tool, we can click and drag the geometry. Then we can also use Control in Windows, or command and Mac, to add additional profiles. We'll set the width to one, and rather than having it extend beyond or go to next, we'll use the depth of 1.2 millimeters. This builds this grill very quickly. And now, we have the primary detail geometry for the part. Next we'll need to add specific features that will help with the manufacturer of this part.