Add ribs and plastic supports. In this video, we'll use rib and web. In Fusion 360 we want to get started with the supply data set, gear reduction housing- molded. We want to expand the sketches folder and note that we have a few sketches, web sketch Rib 1 and Rib 2. Let's first take a look at Rib 1 and Rib 2. We're going to use these sketches to help create some additional features for this plastic-molded version of our gear reduction housing. You'll notice as we look at them, that we do have some reference geometry and in this case we have this closed region. I'm going to get started by first going over to create. We want to create a rib. First, we need to select our curve. If we take a look at selecting just this angled line and we modify some of the values. For example, the depth option could be to next or depth and then we modify some of these values, we can begin dragging these out and take a look at the result. You'll notice when it's set to next and we flip the direction, it's going to create a rib that goes all the way down to the rest of the solid body and it wraps around the cylinder. Let's go ahead and try to add another one. We'll say, we'll repeat the process by going to create and rib and we'll select the other geometry. We're going to set the thickness to four millimeters again. Once again we'll flip the direction, noting that it is wrapping around that cylinder. This is a great way for us to add these different types of supports by simply using a single line reference sketch. It has the intelligence to wrap itself around the curve geometry and it's automatically combined to the rest of the solid model. Let's take a look at another tool that can be helpful called web. We're going to go to a back view. We're going to go to create and select web. First, we need to select the curve. I'm going to select one of these edges, and I'm going to enter a value of four millimeters. Notice how it automatically extends that sketch out in both directions. If I hold down the control or the command key and I make other selections, note that it's able to add multiple selections to this. Even we can grab the circular edge, noting that it's grabbing all of the rest of the geometry. However, when it intersects other solid geometry, we will need to have additional sketch entities in order to complete the rest of that web. When we take a look at the results, this is a very quick way for us to have a sketch that isn't completely defined by surrounding geometry and we allow the software to extend it out completely to the rest of the geometry. I do want to note that there is another tool that we can use. If we use extrude, we have an option called thin extrude. When we use thin extrude, we can select a single line. We can use a wall thickness value. In this case, if we set this to four millimeters equal to what we were using before, and we set it to center, notice that it's creating a very similar option. However, when we're using extrude, we need to be mindful of the fact that it's not going to automatically extend to other solid geometry. This could be a great option because it does open up the available option to set a draft or a taper angle. If we set the taper angle, this will allow us to create a tapered body. However, the rib and web tools do not allow us to apply that taper or draft during the creation. If we need a draft on these features, we would need to come back, use modify, select draft, and pick the areas that we want to draft. Again, the first thing that we need to do is select the pull direction. In our case it's going to be the XZ plane. Then we need to select the faces that we wish to draft. In some cases, you might need to hold down Control or Command to make multiple selections and work your way around the model. If you make the selections and there are any small gaps, you might potentially have an error. For example, here, we need to make sure that we select all the small areas all the way around and then we can apply draft. Once again, keep in mind that using tools like rib and web can be extremely helpful when we're creating plastic parts and we need those additional structural features. However, we do need to be mindful of the fact that draft is not applied and we will still need to go back and use the draft tool to make sure that we do have the appropriate amount of draft or taper on all the required features. From here, let's make sure that we do save this design before moving on.
