 I'm going to be modeling this part, which is supposed to be a chess bishop. And it doesn't look like most bishops, because most bishops would have a longer top. Maybe this is, let's call this the head, just for agreed upon nomenclature here. The head of the bishop is normally taller and stretched out a bit. So if I were to model this a little bit more correctly, I would use probably an ellipsoid. But for the purposes of this being a relatively approachable example, it is a sphere. And this actually looks pretty intimidating when you open it for the first time. You see lots of arcs, lots of dimensions, but when you get down to it, it's not that bad. Geometrically speaking, the main part of the bishop is actually just like five arcs and a couple of lines. So we're actually going to be modeling this using two features. The first feature is going to be a revolution, and that'll be defined by a sketch consisting of half of a cross section from the front view. And then we will create a cut, a linear cut from a sketch on the front plane in order to match the part that's shown here. So if I jump over to SOLIDWORKS and create a new part, I'm going to start with a sketch on the front plane. Now I'm going to arbitrarily decide that the origin of my part will be the bottom center. And then I will move all my lines relative to that origin point. So I will start with the basic lines representing the rough shape of the bishop. So I will add a horizontal line, let's try that again, a horizontal line from the origin, then a vertical line, then a jut in, and then an angle line up. And I'm pretty much out of simple straight lines. Now I start venturing into arc territory. And I personally think that in this particular case it's actually easier to draw whole circles instead of arcs and then to trim off the parts that you don't need. Trying to draw this as a series of arcs just makes it a little bit more complicated and it's harder to recognize the patterns and kind of where the tangents appear. But before I launch into circle territory, I'm going to add my axis of revolution just to make it a little bit easier to kind of visualize what it's going to look like. So I will add a construction line of infinite vertical height starting from the origin. There we go. Now I have my axis of revolution, I'll add some circles. So there'll be one circle representing this surface, one circle representing the, I don't know if this is the head of the bishop, this is the hat of the bishop, this is the scarf of the bishop, this is the neck of the bishop. Okay, are we all in agreement on that? So one of these circles will represent the neck of the bishop, one of the circles will represent the scarf, one of them will represent the head, one of them will represent the hat. One of them will represent the ball on the end of the hat, I guess. So I need five total circles. So I'll use the circle tool starting from the center, and I will make one, and then two, and then what, three-ish, and then four, and then five. So I've recognized that these two circles are probably going to be coincident with this center point of that circle, so I've drawn it that way, but the dimensions will show us whether we're right or wrong, so we can get rid of that coincident if we have to, but let's begin with those. Now I will start to dimension, and I'm going to start like I drew. I'm going to start dimensioning from the bottom center, so I need to know this distance here first. And the way that I do that is by looking at this very scary looking top view. There are a lot of diameters given here. The relevant one here is the outermost object line. That has a diameter of 1.35 inches, which is a number that I won't remember for long enough to actually make it into SolidWorks. If you look at the bottom of the front view here, you see how this point is vertically aligned with these two points. So that diameter of the outermost object line could represent this distance here, this distance here, or this distance here. So that was 1.35. Oh yeah, 1.35. So I'm establishing a radius instead of a diameter, so I will use half of 1.35, which I will allow SolidWorks to do that math for me. And then I can't add a vertical distance of this yet. I'm going to leave that for a little bit later. I know that you're probably concerned because you can't see that on the front view, but that will fix itself later on. We'll come back to that, I swear. Then I'm going to add the angle here of 45 degrees, and I will furthermore make sure that SolidWorks knows these two lines should be vertical from one another. Cool. And I double-click to exit my sketch for no reason in particular. I'm going to jump back into it. And now I will add dimensions for this circle. The center of that circle is vertically 1.3 inches away from the origin, so I will use the Smart Dimension tool. And if you noticed when I was dimensioning that angle, Smart Dimension is, like its name would suggest, pretty smart. So if I click on two lines, it'll try to figure out what dimension I'm referring to. And so if I click on the center of this circle and then the center of this origin, depending on where I move my cursor, I can dimension a couple of things. So I could dimension off this line if I wanted to, but I'm doing it for the origin just for the sake of demonstration. So from the origin, if I drag my cursor over here to the right, I get a vertical distance. So that should be 1.3 inches. And then if I click on those two points again, I can add a horizontal distance, which is shown on the side view of 1.7 inches. Now I'll add a radius. It's shown as 1.5. I think SolidWorks will make me dimension a diameter. So that would be 1.5 times 2, which on most days is 3. And I doubt, wow, how did that end up being? Let's try that again. 1.5 times 2 is 3, not 4.5. There we go. That neck is looking right. So next up is the scarf, I believe. Let me drag my circle down to where I expect it to be, just to make that a little bit easier. That scarf has a radius of 0.1 inches. So a diameter of 0.2 inches. Wow, that's pretty close. Good eyeballing me. And then the head of the bishop is not a radius of 0.05. That would be this circle down here in the cut. So I need to jump back up to the scary top view. And I recognize that the head of the bishop is going to appear as an object line. From the top perspective, this bishop will have object lines here, here, here. I mean at the cut and then here. So in this case, it's going to be the object line that appears second from the outside. That's going to be the relevant diameter. So second object line from the outside, from the outside, from the outside, is the radius of 0.5. Awesome. So a diameter of 1, I think, 0.5 times two. Yes, one inch. And then I'm going to give this a radius, which of course is shown on the front view that has a radius, the hat, the base of the hat or whatever is 0.5. So that dimension is going to be a diameter of also 0.5 times two, which I think is still one. And it is indeed still one. Cool beans. Lastly, the ball on the tip of the hat, which is shown on the top view, and this is again going to be an object line, and this is going to be the smallest object line as visible from the top. So the smallest object line is a diameter of 0.28125. Nice round number, 0.28125, 0.28125. There we go. Cool. Now I have my diameters, my circles, and this one is positioned so I can start to position the rest of them. So the first thing I'm going to do just for my own sanity is get rid of this coincident, because that's one that I'm kind of predicting. So I don't want to bind myself to it. I want to make sure that it's free to move around. And then if I think that it's coincident, I can add that back later if I need to. But I actually think that solid works, geometrically speaking, this bishop should end up pretty good. So that is going to be a height of 1.85, and that's going to be this distance here. That's 1.85. And then the next circle is vertically 2.25 up, so 2.25. And look at that, look at that on the circle. Pretty much centered, pretty close, not bad. Good job, geometry. And then my hat is tangent, and the hat is also going to be tangent to the axis of revolution. So I'll add that now. So I'm shift clicking the circle and the axis of revolution, I'm adding the tangent constraint. Now that one's fully defined, last but not least, is the ball on the end of the hat, which is vertically three inches up. Okay, now I noticed that I may have been wrong about that tangent. So I was given a dimension here, that's 2.875, that's referring to the intersection between the ball at the top of the hat and the base of the hat. So that's going to supersede the assumption of tangent between the circle and the center line. So I'll get rid of that tangent and do this properly. Smart dimension, origin, this intersection here. So that I'm going to have to do a little bit differently. I'm going to have to clarify that I'm defining a new point. And I'm going to tell SolidWorks that there is a point at the intersection of those two circles. So I create a point. And then I draw a point. And for the sake of demonstration, I'm going to draw that point out here in space. I now have a point. Now if I shift click that point and this circle and I tell it to be coincident, then I shift click that point and this circle and I tell it to be coincident. Now that point is on both circles, therefore it is at the intersection. So I can move that around and adjust the position of that base of the hat thing. So I'm going to use smart dimension, click on that new point, click on the origin, give that a dimension of 2.875, 2.875. And look at that. Pretty close to tangent, but for the sake of round numbers, we're using that distance. Cool. So now I have some fully positioned circles. Now I'm going to go use my trim tool to get rid of the extraneous parts of the circles. And power trim is the easiest way to do that. Power trim, you just kind of click and drag in any line that you go across and your click and drag is removed. And SolidWorks tries to figure out like the two intersections on either side of where you clicked through, and then it removes the things between those two intersections. So if I click and drag through this circle, you'll notice it got rid of that big part of that circle. The reason that this little line is still shown is because that's used for dimensioning. It's for showing the diameter of 3 inches. So like if I exit my trim tool and move this around, you'll notice that line disappears. It's not a real line. So I will carefully use my trim tool and get rid of some more lines. Say that line, don't need that, and oh, whoops, a little too heavy handed. Let's try that again. That line, and that line, and that line, and that line, and these two lines, and then that line, and then that line, and that line, and that line. There. I got rid of all of my extraneous lines. You'll notice that I also kind of broke a couple of my constraints. That's okay. I can go back and fix those. So one of the constraints is the fact that I think this line doesn't know, yeah. So I need to clarify that position again. So now that it's able to be moved around, I'm going to clarify that this head is going to be coincident to this point. And then I'm going to make this point, that's the center of the scarf, also coincident to this arc. So I've basically restored the fact that these two circles had once been touching. So by making it coincident, making this center point coincident, I'm telling it that this center point and this line should touch. And even though they don't touch, I mean they would if this line were continued. It intersects with the function of that arc. Now I believe all of my lines are fully constrained. I have the basic part, except for this thing we talked about, I need to bring this back. So I'm actually going to be giving this a horizontal distance, not a vertical distance. So you see I can drag this around. And if I give it a horizontal distance, that'll bind its vertical distance as well. That's actually shown, I believe, in two places. On the top view, you can see that's the second line, I think, yeah, 1.25. It's also shown down here for a little bit of over dimensioning, so 0.625 radius or a point or 1.25 inch diameter. So I'll use this distance, 0.625, all smart dimension from the origin again, and then this point, and I'll drag it down to give it a horizontal dimension. And that was zero point, let's try that again, 0.625 inches. Now I believe I have a fully constrained sketch. So for good practice, I will add a line down the center to close the region. Now with much ado, I can create my revolved base. And look at that. I've got a good looking bishop. So if you just tried that at home, and you were unable to get it to work in a single click like I just did, you may have had to go in and close your sketch somewhere. You may have had too many lines. Solidworks needs to know what the region is that you want to actually extrude, the thing that you want to make into a solid. If you had too many lines, you may have had to go in, click this box, and then click that region. That's a thing that you may have had to do. But because I got rid of all of the extraneous lines, Solidworks knows the region that I want to extrude. So that was an advantage of doing it the way that I did. But regardless, we have the shape of our bishop. Is that a good looking bishop? I agree it is indeed. Now I'll add my cut. So I need that cut, this slot, to be visible directly from the front view, which means I'm going to be drawing it on the front plane and then extruding the cut. So I will create that basic shape on a sketch on the front view again. So I will go up to sketch, create a new sketch, select the front plane, and now I recognize that I begin with a circle again, and that circle shares the same center point as the head of the bishop. So if I kind of hover over this arc, you'll see that nothing appears. Isn't that nice? So I will just add a circle in the center arbitrarily, and then highlight the circle and the arc out here. And then tell Solidworks I want those to be concentric circles. So concentric means sharing the same center point. And that should be good. You'll notice that if I vertically align it here, that breaks. And that's because I actually, in my original sketch, yeah I know Solidworks, it's a broken dimension, it's fine. Trying to prove a point. You'll notice that because I told Solidworks to have this arc intersect at this point, that the center of that arc isn't exactly over the vertical point. So the center of that arc, according to the dimensions of the drawing, is not above the origin, it's not vertically aligned. So this isn't actually a sphere, it's a slightly wider sphere. So going with concentric circles here is not actually the best way to do that because, I mean, if I were to, let's jump back to the other sketch, I know it's still broken. I'm trying to prove a point, Solidworks, give me a break. Okay, so by defining it to be concentric with this arc, I am now not concentric with this arc. So I have the option of being either concentric with this arc or this arc, but not both. And neither one of those is going to be vertically aligned. So let's approach this from another angle. Maybe instead of being concentric to one of those, maybe it would be better to be centered on the head of the bishop to say, well, if I want this to be vertically aligned, you'll notice that it didn't break anymore. And maybe I want it to be positioned such that the center of the arc, the center of the circle here is vertically aligned between these two lines, something like that. Or, better yet, I'm actually going to use a point again. If I use a point again, I'm going to tell Solidworks that this arc and this point should be concentric. So by highlighting that point and shift clicking this arc out here, I've told Solidworks to create a point at the center of that circle. Now if I repeat that process, again, I'm adding an arbitrary point, I'm highlighting this arc out here, shift clicking this point, making them be concentric. Now I have two points representing the center of both of those arcs. So now if I were to add a construction line between the two, I can add this point, which is the center of the circle that I'm creating. And I can shift click this line and make that be midpoint. And that is the best way to center that circle. How's that for convoluted? It would have been much easier to have interpreted the engineering drawing as having this be centered over the line and then not having this line coincident to that point. Let's jump back to the other sketch here. I have a circle now, completely logical circle. I'm going to add some lines because circle plus some lines is the shape of the slot that I want to cut. So I'm going to add some lines out here. I'm going to add a construction line and put it from this point right here, too many points too close. And then I'm going to tell Solidworks to make these three lines parallel. Let's try that again, these three lines parallel. And then I'm going to dimension this line and this as having an angle of 45 degrees. Why that surface you ask? Because that was what was shown in the drawing. And then I am going to have to close off this sketch in order to create the cut. So I'm going to add another arc here. And in this case, I'm actually going to use an arc instead of a circle. So I'm using a center point arc. And then I'm using the center of this arc over here, which again is represented by this point. And then I'm connecting these two points here. So you know what, just for demonstration, I'll just make this arc out in space. I'll highlight this arc, and then highlight this arc, make them be concentric with it, which they already are. And curadial, make this point and this line coincidence. And that should result in these two being pretty much coincident, but I'll add the constraint just for good measure. Now that I have an arc completing the sketch, I can trim off this extra bit of line. And then trim off this extra bit of circle. Now I'm going to add a diameter of the circle, which we can finally use this radius here, 0.05 inches, 0.5 for a radius. And now I have a fully defined sketch with which to cut. So I'll exit my sketch, I'll go to features, I'll do an extruded cut. And I want it to cut all the way through in both directions. So I use the through all, I click OK. And now I have my shape. So if I look at it from the front, that matches my drawing pretty well. So I'm going to create an isometric view and then export my part.