 I'm going to be making this rocket, and I recognize that I can split it into a couple of different components. I'm going to start with a revolved base to make the fuselage shape, this center body part. And then I'm going to create a single fin and extrude that using an extruded base, and then make a pattern of them around the center of the rocket to create the three fins that I need with an offset of 120 degrees each. And then I'm going to use a revolved cut to remove this center part. So if this were a model rocket, that might be where you put the rocket engine, although this is 96 inches tall, so maybe it's just a really, really big model rocket. Anyway, I'm going to start with a sketch representing half of the cross section of the main body of my rocket from a front view. So if I jump into SolidWorks and create a new part, I can create a sketch on the front plane, and then I'm going to be making the basic geometry first and then going through and dimensioning it. So I recognize that I want to have a vertical line up the center, and then an angle down, and then a vertical line down, and then a little jut in here for the nozzle, and then an angle down, and then a horizontal line to complete the sketch. I'm going to arbitrarily decide that the origin point of my model should be the center of the bottom of the nozzle, so I'll be using that. Now if I jump back into SolidWorks, I can add a, let's try that, a line up the center, then an angle line for the nose, a vertical line for the outside, a jut in for the nozzle, and then an angle line and a horizontal line. That's my general shape. Now I can go through and add dimensions. So I know the height of my rocket, or rather the height from the bottom of the nozzle to the tip, which is 96 inches, so I will add that here, that is 96 inches. Then I know that my nose should have an angle of 50 degrees. I'm drawing half of that, so that angle should be 25 degrees. I'll use the Smart Dimension tool, and that will, if I click on this line and this line, that'll figure out that I want to dimension an angle, so I'll click there, and then make this 25 degrees, because that's half of 50. Next I know that my nozzle should be 6 inches tall, so I can dimension from this vertical line to this vertical line, tell it that should be 6 inches. Now I will add my diameters of the rocket, which are going to be radiuses here. So if I look at my top view of my sketch, I notice I have a lot of diameters, but the first one, the outside one, is 16 inches, which means that this radius here should be half of 16, which on most days is 8. And if you didn't want to do that math in your head, by the way, if you just type 16 slash 2, it'll do the division for you. Next I notice that I need diameters of 14.5, 14, and 12. And if I look closely at these arrows, I see that the second line is 14.5. And if you picture how this would actually look from the top, that second line is going to be this distance here. That's going to be the line created by the top of my nozzle, therefore I'm going to make that half of 14.5, which is 7.25, and then I'm going to make the bottom of my nozzle 12 inches in diameter, which would be a 6 inch radius. If you're having trouble recognizing the distinction between these hidden lines, if you look at it from the front, see if I can get down there, if you look at it from the front, you can see that this edge of the nozzle is further out from the center than is the inside surface of the cutout. So the second line you see from the outside, from a top perspective, is that top of the nozzle. So now I have my dimensions for the main body. Everything is black, which means it's fully defined. I can add an axis of revolution and create the part. So I'm going to create this as an infinitely tall vertical line from the origin to make sure it's centered. And now I can go to Features, Revolved Base, and I get my basic rocket shape. Cool. Now I'm going to add a fin. So I'm going to add the fin on the front plane because I want to make my model match the model indicated in this drawing. So the first fin here on the right is visible perpendicularly from the front view, which means it would be drawn on the front plane. Then when I create the pattern, I end up with fins that aren't aligned to any of the primary planes. So if I jump into the front view and create a sketch on the front plane, I can create the shape of the fin. So I'll have a line, and then a line, and a line, and then a line. How's that for a good fin? Now I can add dimensions. So I need the angle at the top to be 25 degrees. So again, I'll use the Smart Dimension and then click this line, and this line, and tell it that I want it to be 25 degrees. And you'll notice that that brought all the other lines around, which kind of broke the shape of my fin, but it's okay. I can bring it back by quitting the Smart Dimension Tool and then dragging this point over to where I want it to be. I'm going to tell Solidworks I want this line on the outside to be vertical. That way it won't get all kiddywampus again. And I'll add another angle at the bottom, which was 45 degrees. And I'll dimension a width, which I believe is 10 inches, yes, 10 inches. And I will dimension a height from the bottom. So I know that the bottom of the fin is going to be 3 inches below the bottom of the nozzle. So if I click this point, and then hover over the bottom of the nozzle and select that face. I can dimension this as being 3 inches. And then I need to add in the fact that the height of the outside of the fin needs to be 21 inches, and that should fully define my fin. So 21 inches. And there we go. The fin is turned black, which means it's fully defined. But here's the problem. If I were to just create a base extrusion now, I would end up with a fin that didn't actually touch the rocket. If you look at it from a top view, you see how the outside surface of the rocket is a circle? I mean, it's actually a circle. Solidworks is showing a preview view as a polygon here, but it's actually a circle. This is just to save video memory, I believe. It's trying to make it easier to render. Whatever the case, if I were to extrude linearly here, I'm going to be going away from the body of the rocket. I want the fin to be touching the rocket the whole time it's extruded. So the easiest way for me to do that is to actually bring the inside edge of the fin inside the body of the rocket. When I create the extrusion, Solidworks will actually join all the bodies anyway, so it doesn't really matter. So if I go back to my sketch, I'm going to first remove these two coincidences, which I do by clicking on the green box and hitting delete. And now I'm free to move the fin left and right. So first of all, I'm going to get rid of this line that I didn't know was there. Interesting, I must have clicked a couple too many times. And now I'm going to start my fin inside the actual body of the rocket. That's why I chose to create the cut, representing the inside of the rocket after the fin. That way, if I extrude the fin too far, the cut will remove that material as well. So I'm going to kind of arbitrarily set the inside of my fin as being, I don't know, an inch inside the outside surface of the rocket. And now I need to fix the rest of my dimensions here. So first of all, I need to specify that that 10 inches is no longer from the inside of my sketch to the outside of my sketch. That is from the actual outside surface of the rocket, which again, I hover over that and click and then click on this line. And now I can add the 10 inches. There we go. That brings it back. I could have also dimensioned from this line to this line and made that 11 because it's 10 plus one. But this way is a little bit easier, a little bit more elegant, my opinion. It doesn't actually matter what dimension I use here. I could say one inch. I could say six inches. It's actually okay because again, I'm cutting after I create the fin. So the cut will remove any extraneous material that's going too far into the inside of the rocket. For the moment, let's just stick with one. Now I have a fully defined sketch. I can go to features and create an extruded base. And I need this extrusion to happen symmetrically. So I'm going to use the midplane. And I need it to be a total thickness of 0.75 inches. So you see this checkbox? This is merge result. That's what I was referring to earlier. Solidworks is going to join the bodies. And there we go. We have a fin. So even though Solidworks is showing this again as a polygon instead of a round surface, it actually is behaving correctly. So there isn't a single gap at the edge of my fin. Everything is good. Cool. Now as opposed to trying to draw two more fins and then extrude them, I'm going to copy this one fin and create a pattern. And the type of pattern is going to be a circular pattern, not a linear pattern. Because I want it to go around the circular surface of the rocket. So if you click on the arrow below linear pattern, you have a couple of extra patterning options. I want to use circular pattern. So within circular pattern, I have a couple of boxes. This box that's currently highlighted is where I would select my extrusion that represents the fin. But you'll notice nothing is happening. That's because I also need to specify something in this box. That is the axis around which to revolve to create the circular pattern. So I don't actually have a nice middle line. You know, if this were a sketch and I was creating a revolved extrusion, I would create a construction line there down the center and revolve around that. But I can't just use a construction line here. I can't use a line within a sketch. I need to use the three dimensional equivalent. Which, if I exit out of my pattern here, is an axis. If I go up to reference geometry and click on axis, I can define an axis on my part for reference. So I'm going to be creating an axis down the middle of my rocket and I'm going to be revolving around that. So when I click on axis, I have a couple of options. SOLIDWORKS is basically saying, hey, where do you want that axis? And I have a couple of ways to tell it exactly where. So the first option here is I could select a line that already exists on my part. You know, if I were to select this line on the outside of my fin, I could make that be an axis. But that isn't helpful here. I've got other options like two points, which is where I could select two points on my sketch or excuse me, on my part. And SOLIDWORKS would create an axis between them. I have point and face, which I don't really have any convenient examples of here. I guess maybe this one, I could select this is the face and then this is the point. And SOLIDWORKS will create an axis that is perpendicular or rather normal to that plane and intersects the point that I selected. That would actually work here, but it's not the one that I would prefer to use. I have cylindrical face, which if I click on a face of a cylinder, will create an axis down the center that again would work here. But my favorite option for this particular circumstance is the two planes option. SOLIDWORKS will create an axis at the line resultant from the intersection of two planes. So if I were to click the front and top planes, those intersect at a line that extends horizontally here. So because my origin is at the bottom center of the nozzle, that horizontal line is extending away from the bottom center of the nozzle. So in this case, if I choose the front plane and the side plane, the right plane, the resultant axis is right down the center of my part because I revolved it around the origin. So that's perfect. That's the one I'd like to use here. Now I have an axis. So if I jump back to a front view for convenience and I go to circular pattern, I'm going to select that extrusion representing my fin again. And then up here in this box, I'm going to select that axis that I created. Now I have some options here. For example, right now I have equal spacing ticked. That means that it'll take the number of iterations in the pattern and space them equally among this angle. So right now it's taking that extrusion and creating three of them that are equally spaced around 360 degrees, which is actually what I want. If I had unchecked equal spacing, I would have to specify an offset between the fins. So here I could say 120 degrees and I would end up with the same result. But by making this be 360 degrees and equal spacing, I have kind of a convenient way to add or subtract fins. If I wanted to make the worst rocket in the world, I could add just dozens of these fins and end up with something that looks like a heat sink more than a rocket and would probably fly straight, but not very far. But if I jump back into that pattern, which I did by right clicking and clicking on edit, and make this be three, now I end up with the number of fins and the offset that I wanted. Three fins spaced equally around 360 degrees. I'm very nearly done. I now need to add the cut representing the middle section of the body. So the cut representing these hidden lines here. And again, I created the cut after the fins so that if the fins extended too far, the cut would remove them. And I'm going to use a revolved cut because of the rotational symmetry. So I'm going to be drawing half of this cut and then revolving it around a center. So I'm going to create another sketch. I could do that on the front or side planes, but I'm going to do that on the front because if it ain't broken, et cetera, then I'm going to draw the basic shape again, which is going to go vertical line up from the origin, over, down, add an angle, and then horizontally at the bottom of the nozzle. Then I'm going to add a relation for this angled line that it needs to be perpendicular to the outside of my nozzle. Sorry, parallel to the outside of the nozzle. And now I can start to dimension. So I read that I need, I read that I need a half inch so the nozzle has a thickness of half an inch. So I click on this line and this line with the smart dimension, tell it to be half an inch. Next, I'm going to add a height. So over here in the front view again, I see that the height of that cutout section is 60 inches. So this line needs to be 60 inches tall. Then I can add a radius distance, which I go back to the mess of a top view I have here and read, well, that hidden view. That is going to be not the first hidden line because that's the top of the nozzle. It's the second one now. And that has a diameter of 14 inches. So that 14 inch diameter would mean that I specify a radius here of seven inches. Now that sketch is black, I think. Yeah, it's fully defined. No, definitely fully defined. He said confidently. Oh, I see. I want to make sure that that center line that I drew is coincident to the origin and not the axis. So I have a sketch now representing my revolved cut. And then I'm going to add a construction line. Again, infinitely tall and vertical to represent the axis of revolution. And the reason I'm doing that instead of just using the axis that we created earlier is because I like the geometry in my sketch to be kind of contained as much as possible. That way I can mess with the axis if I wanted to and it wouldn't interfere too much with my sketch. Then I go up to features and revolved cut this time. And then I'm going to use the contour defined by this region and then accept that cut. And you notice how nothing changed? That's because the cut is inside. So if I jump in to a bottom view, I can see that region I just removed. And to make sure that it looks correct, I'm going to go back to a front view. I'm going to change my view settings to hidden lines shown. Now I kind of have this x-ray view. And I see that that looks pretty good. That is pretty much exactly what is on the drawing. Excellent. And I've completed my rocket.