Creating a hollow cavity - Fusion 360 Tutorial

- [Instructor] Hi, everyone. In this lesson we will turn all of our surfaces into one and into a solid body. But first, let's make sure that our workspace is in patch mode. Inspecting our bodies, we have three surfaces. Let me turn on body two, and obviously body five is not needed. To be organized, let's remove this one. We have the option to delete, but the problem with delete is it may cause problems if the feature is referenced by other feature in the timeline. So a good option for us to be organized is by right clicking and selecting remove. Now the remove command simply removes our body into the bodies folder. Selecting remove and turning on the visibility of our body two. Let's now patch the holes. Going to create, selecting patch, selecting this edge, continuity, connected, operation, new body, hitting okay. Repeating patch, selecting this edge, and hitting okay. And from here we can now head to modify and select stitch, making sure that under select, window selection, this turned on. Creating a window selection, left click and hold, release. Let's leave the defaults. Operation, new body, and hitting okay. Notice in our bodies folder, it now turned into a solid body. Next, let's create a cylindrical protrusion here that will mate together with our plastic cap. I'm going to hit C to grab our circle, select this face as our sketch plane, and, instead of creating a circle, I will utilize our offset tool. I'm going to hit escape, but first, let's project this circular edge and hit okay. I'm going to go to top view. My intent here is to shell out this body having a two millimeter wall thickness. Hitting O, selecting this edge, let's grab this slider inward, and I'm going to key in negative two, finally hitting okay. Let's hit stop sketch and turn on the visibility of our canvas. Hitting E for extrude, selecting this circular profile, moving our arrow up, going to front view, pulling this arrow down, and let's key in 10 for distance. Operation join and hit okay. And before grabbing our shell tool, let's add fillets hitting F, selecting this edge and this edge, the radius to be five. Let's add another selection, this time selecting this edge and this bottom edge. Radius to be two. Leaving the defaults and hitting okay. And before shelling, we're going to turn off the visibility of our canvas, hitting S for model toolbox, and typing SH, selecting shell, let's exclude this face. Selecting this face, and our inside thickness, keying in two, direction inside, and finally hitting okay. To end this lesson, let's add a thread on this surface. I'm going to go to create, selecting thread, selecting this face, thread to be isometric profile size 33. For the designation, let's change this one to M33 by two. Class, 6g, direction, right hand. Uncheck remember size, and, instead of having a graphical representation, I want this to be modeled. Finally hitting okay. And in the next chapter we will finally create our cap. See you there.