Create a revolved solid

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Create a revolved solid.

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In this video, we’ll create a revolved body.

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In Fusion 360, we want to carry on with our gear reduction housing solids.

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We've already added geometry to the front cover that allows us to hold a 5 millimeter thick bearing but we need do the same to the back.

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So first let's go in and let's rename some of these bodies.

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Body 5 will be front cover, Body 2 will be front housing and Body 1 will be back housing.

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Now we want to focus our attention on the back housing, so we're going to hide the front cover and the front housing.

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We're going to use a Revolve to create the geometry to hold the bearing on the back side.

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We could do this with another extrude, but let's take a look at this other tool.

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We're going to select sketch and we want to select our YZ plane.

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I'm going to use the Slice option so I can take a look at the geometry on the inside.

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I'm going to begin by sketching a line, going to drag this out to the right hand side and then hit Escape.

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Select the line and I'm going to make it a center line.

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Next I'm going to rotate the housing slightly, go to Create Project/Include and Intersect.

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I want to grab some references from the surrounding geometry such as the inside diameter of this bore and the outside face and say, OK.

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From a right view now I have some geometry that I can snap to.

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We're going to start with the Line tool noting that the hole here is already 21 mm.

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So we're going to carry this out, come in toward the center and then begin drawing and dragging out until we have this L shape.

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Now we're going to use our Dimension tool to apply some dimensions.

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The distance between these two edges is going to be our housing thickness.

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So we're going to start typing housing and then select the Housing_Wall_Thickness parameter.

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We're going to do the same thing on this end, once again beginning to type in housing.

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Next, we need to have the diameter of the opening, which is going to be 10 mm.

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Because we defined the construction line as a center line, noting that it already gives us this as a diameter value and not a radius.

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So I simply need to enter 10 and say, OK.

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Next we need to make sure that we have 5 mm for the bearing.

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So we're going to come in and manually add that 5 mm and then finish our sketch.

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Now that we have our completed sketch, we can go to Create and Revolve.

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Because that was our only closed sketch profile, it automatically selects it for us in the center line, creating the geometry.

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We're going to join it with the surrounding body and then we want to bring back our front housing and our front cover.

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We'll go to Inspect, Section Analysis and we want to use the left click to select YZ.

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We're going to view this from the right and we'll say OK to create our section view.

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Now, we're beginning to see the shape of our housing and in this case, you can see that we have area for the large gear on the right hand side,

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area for the smaller gear and all the idler gears on the left hand side,

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and three positions for bearings that have a 21 millimeter OD, 5 millimeter thickness and then they have a 12 millimeter ID.

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This will be able to support the 10 millimeter input and output shafts that we need.

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And also note that one of these gears will also contain a bearing to help support the other,

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because we need to make sure that the shafts are concentric but not connected.

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Let's navigate to a home position, expand the Analysis folder and let's hide our section view.

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Let's make sure that we do save this design before moving on.