 I'm going to be trying to make this mug, and there are a couple of ways I could approach that, but all of them pretty much have the same thing in common. I'm going to be trying to generate the center part of the mug and then the handle separately. The center part of the mug could be done using a shell or a thin feature, but for the moment I'm going to be drawing the inside and outside surface on the same sketch and then revolving them around a center axis to produce my shape. Then once I have my shape, I'm going to draw a cross-sectional view of the handle on the front plane, and then I'm going to extrude it to create the handle. So if I jump into SOLIDWORKS, I'm going to be creating a new part, and I'm going to start with a sketch on the front plane. So I need to draw half of what the cross-section of just the center part of the mug would look like. So the basic shape of that is going to be a line, and I'm going to start that at the origin, a line, and then I need an arc. So I'm going to draw a, let's go a center point arc here, and then I'm going to draw another line. So that'll give me my basic shape. Now I can start to constrain and dimension that shape. So I know that the inside is going to be the same basic shape, so if I dimension and constrain the outside, I can just copy that to make the inside surface. So let's start with that arc. That arc needs to have a radius of 4.5 inches. So I go up to Smart Dimension and then click the arc. I can give it a radius, and I'm going to say 4.5 inches. Then I can also recognize that the outside of my mug here, that, or should I say the outside top part, is going to have a diameter of, let's see here, 3.5 inches. So I'm going to make a construction line in the center to represent my axis of symmetry, and I'm going to make that infinitely long and vertical, and then I'm going to constrain that to the origin because I missed that click. Now I can tell Solidworks that this top outside part of the mug should have a radius of 1.5 of 3.5 inches. So 3.5 divided by 2. Cool. Broke it already. Now I'm going to be dragging in this point down here in the corner. So I'm going to exit out a sketch dimension, or Smart Dimension, and then shape this a little better. Then I'm going to click this line and shift click the arc, and tell Solidworks I want those two features to be tangent to each other. I'm going to give it the horizontal distance of the bottom part of the mug, which I know from the sketch has a diameter of 1.75 inches. So 1.75 divided by 2 would give me that radius. Now you see how the entire sketch is fully defined except for this blue dot up here. That blue dot, if I drag it around, is not vertically constrained. So I should add a height to my mug, which is shown over here in the side view. That height is 4 inches. So if I click the dot and the line, and then drag that out to the side, I need that to be 4 inches tall. And that's the basic shape of my mug. Now I'm going to duplicate those. So I'm going to repeat the same. I guess I could repeat the same process, generate an arc, generate a line, generate a line, or if I wanted to, I could highlight these three lines that I just drew and use the offset entities tool as kind of a shortcut. So I want to make those lines be duplicated a certain dimension in. So I'm going to look at my part here and I see that I want the thickness of that wall to be 0.085 inches. So I want this to be 0.085 inches. And if I hit OK, it will duplicate those lines, create a copy of them 0.085 inches in. So I'm very nearly there. I need to close this sketch by adding a line at the top to represent the actual top surface of my mug. And then I'm going to close down here. So that solid works knows the actual region that I want to revolve around this axis. If I left that open, it would have had to guess that I wanted the axis to be the center, sort of like using the fill tool and paint. You know, if you don't have that region closed, it could fill everywhere solid works to get a little bit confused. So I'm going to use features. And then I want to use the revolved base to create my 3d part around that axis of revolution that I already defined. That was my construction line. And then I want to select the contour to revolve. And I'm going to click this region and hit OK. And I'm now looking at a mug without a handle. So that's okay, we're starting to get a handle on this. So if I look at it from the front view, the region I chose the front view is because I'm going to be drawing in the front plane. The reason I know I'm going to be drawing in the front plane is because I want that handle to be visible from the front view. If looking at it from the side, I should see just a rectangle. So on that front view, I'm going to add a sketch to represent the shape of the handle. And then I'm going to use the extruded base to actually generate the 3d object. So I'm going to create a new sketch. And I'm going to create that sketch on the front plane. Now I know that that handle actually consists of two semi circles. There's this semi circle up here, which has a radius of 1.15 inches. And that starts or rather the center point is right here on the edge of the mug. And at this intersect between the arc and the line that we use to generate the middle part. So that center point will be on the edge of the mug. And then I want it to end horizontally aligned to that center point. Then the second semi circle has a center point horizontally aligned to the center point of the first arc. And that has a radius of 2.15. So I'm going to create those basic shapes. I want to create a center point arc. I'm going to click here to represent the center point of my arc. I'm going to click up here. And then I'm going to create an arc that ends horizontally from the center point of that arc. Now I'll add a dimension. I want that to have a radius of 1.15. Then I'm going to add another center point arc. So I want that second center point to be somewhere else horizontally aligned with that first center point. So I click over here. And then I want the arc to start with this arc and then go down and stop at the edge of the mug. And then I can dimension that and say it has a dimension of 2.15 inches. Then I want solidworks to know that these two arcs need to be tangent to each other. And now you see that line is fully defined. So I can repeat the same process I did earlier. I can highlight these two arcs and use the offset entities tool to create a duplicate of them in a certain direction. In this case that offset needs to be 0.15 inches. So I'm going to say 0.15 inches. And then I will accept that and it'll create that duplicate. So there are a couple of issues here. The first issue is the fact that this region still isn't closed. I need to close this region in order to extrude it. So Solidworks knows what I actually want to extrude. The second thing is that if I were to start this handle at this surface of the mug, like if you looked at it from the top, if I extruded that line away linearly, it wouldn't actually follow the surface of the mug. The mug is round. And if I extruded linearly, I would end up out here in space. It wouldn't actually be touching the mug anywhere but at this center point. So what I need to do to fix that is not actually start my handle at the edge of my mug. I want to start the handle a little bit inside of the part of my mug. So by starting inside of the mug, when I extrude, those bodies will all be combined. And I will end up with a handle that follows the surface of the mug. So I'm going to jump back to my sketch. And I'm actually going to remove this constraint that I added earlier. I'm going to click on that green box. And now that dot has turned blue. And I can drag it around. I clicked on that box and hit delete, by the way. So I'm going to drag it inside. And then I'm going to make this follow that dot. I want both of them to be inside. Now how much inside depends. I really only need enough to ensure that when I extrude, that it isn't outside of the surface of the mug. But just for convenience's sake, I'm actually going to constrain these two points to the inside surface of the mug. So if I change my view style from shaded with an outline, by clicking this button up here, the fifth button from the left or sixth button from the left, and then change it to hidden lines visible. Now I kind of have an x-ray view of my mug. And if I click on this dashed line, that would represent the inside surface of the mug. So if I click on that line, and then I shift click this point, I can hit coincident. And now that dot is actually aligned with the inside surface of my mug. So by starting from the inside surface and extruding linearly, I ensure that I never actually go into the inside of my mug. And I am definitely going to have a handle that is inside the the mug thickness the whole time. The nice thing about constraining it as opposed to dimensioning it is that now if I needed to resize the mug, it's likely that the handle would follow this and not be screwed up. Another way to approach this would be to create a single entity for the big mug, add a handle, and then add the cut after the handle, the cut representing the inside of the mug. If I cut out the center of the mug after I had added the handle, then it would cut out the material of the handle as well. And I wouldn't have to worry about it. But continuing this process, I'm going to click that point, shift click this line, hit coincident. Now both of these two points are on the inside surface. I'm going to repeat that process down at the bottom. I'm going to click this point and then click the line and then click can excuse me, coincident. So let's try that again point line, coincident, and SOLIDWORKS is throwing up an error. So I'm going to remove the coincident and try to diagnose the air here. Let's try that. Maybe the third time is a charm. Something doesn't work just continue to try it until it works for some reason. Great. I'm going to remove this coincident and repeat the process. There we go. Now I have my handle constrained to the inside surface of my mug. Now I need to close the sketch, which on the top part is pretty easy. I just add a line between these two points. Now on the bottom part, if I were to just use a line to connect these two points, then geometrically speaking that line is going to be not quite aligned with the arc that represents the actual inside surface of the mug. And that line in reality would be on the inside of the arc representing the curve of the inside of the mug. So for good practice here, let's create an arc that follows the actual inside surface of the mug. So I'm going to use the center point arc tool again. And I'm going to start my arc from the center point of the arc that represents the inside surface of the mug. So the way I got that center point to appear is just kind of by hovering over the inside surface, and then the relevant geometry kind of popped up. So this dot over here on the left represents the center point of that arc. So if I click that, and now click on one of these points, and then the second point, I now have a fully defined, excuse me, I now have an arc connecting the two points. So I'm going to click on that arc, and now click on the inside surface again, shift click. And I want those two arcs to be curatial and concentric. So they have the same radius and they have the same center point. Now that line is black, it's now fully defined. So if I look at my sketch, I don't see any blue parts, which means that I have a fully defined sketch. Now I can use the extruded base to add some thickness to my handle. I'm going to use the midpoint or midplane extrusion. And I need that handle to be 0.5 inches thick. So 0.5. Then I accept, and I have a handle. So if I switch back to my shaded with edges, then change that to an isometric view, there's my mug.