 Hey guys, Vladimir here with desktop mix. I thought I'd do a tutorial showing my design approach and techniques I use to create this spur gear assembly here. So I've got a few projects in mind that are going to be using this mechanism and I thought I'd start with sort of this basic approach here on how I designed the spur gear and the rack here and my approach to getting them to align so perfectly. So in this video, we'll take a look at that and in the next video, I'll show how I was able to apply the motion you see here using joints and motion links. So all right, we'll get started. And first thing actually I want to show is that I approached this design using components. So here we've got our base and our spur gear and in our rack here. I think you're going to find this model very fun to design and 3D print and also highly educational. Let's jump right in. We'll begin by creating a new design and here instead of starting with a sketch, we're going to go ahead and start by using a gear generator right under the utilities menu here and we can go to add-ins and then script and add-ins. We'll get this dialogue box and if you scroll all the way down, we'll see our Python spur gear generator. We're going to click run and you'll get this dialogue box here. Now don't be overwhelmed if you see all these terms here that you may not grasp the full meaning of. I'm no mechanical engineer here and actually my approach to this was just to kind of play around with the numbers and see what happens, sort of a trial and error here. So the way I started is I looked at this pitch diameter and I have a pitch diameter in mind of the size of gear I want to make. So I started experimenting with the numbers here to see what affects that parameter there. Now you can't directly change pitch diameter, you just can only affect it by changing these other parameters. And I found that the two that affected are the number of teeth and the module. So number of teeth 24 sounded good to me, module. I brought that down to two and that went from a 300 and something pitch diameter to 48 millimeters. All right, that looks good except I've got this sort of message here and I can see my okay button is grayed out. So let's look at what that message says. It says the root fillet radius is too large, it must be less than 1.18. No problem. I could make that happen. The root fillet radius is going to change that to 1. Now the rest of the gear thickness, you can make that whatever thickness you want. I'm going to leave it at 12.7, not sure if that's sort of a default gear thickness or what. Whole diameter, I'll just leave it the same as well. You can always change this by creating a sketch and extruding anyway. But I'm going to not complicate things, leave everything else as is and click okay and there we have it. My gear right there on the origin there centered on the XY plane in this orientation. I can move it if I want but I'm just going to leave it as is. And also one thing I want to point out is that came in as a component. So you can see the little component symbol there and if I expand it you see you've got your own bodies and your own sketches. The cool thing here, if I go down to the timeline and I click the little plus button, you can actually see how this component was made with that Python script. So here if I just walk through the timeline, we've got a couple sketches there, an extrusion, a second sketch here and this sketch actually shows the profile that was made to create the tooth of the gear. So here we see it's generating a bunch of spline points to create that profile and then the next item here extrudes it up and we have a fillet and a circular pattern and then our final sketch here shows that pitch diameter circle here at 48 millimeters. So I just wanted to show that here just in case you were curious of how they made this and you kind of wanted to see an approach on making your own. Okay, that's that. I'll collapse that timeline there and now we'll create our next component here, which is going to be our rack. To do that, I'll click on the top of my browser here, select new component and give it a name. We're going to call this one a rack and then we're going to orient to a top view here as we're looking at it from our view cube orientation. And I'm going to right click, go to move, copy, I'm going to select the translate option here, move object is set to bodies, I'm going to select the body and I want to move this down a certain distance. Now how far do I want to move it down? Well this is very important because this is what's going to determine whether the two gears mesh or in this case the gear in my rack. So the answer to that is you want to look at what that pitch diameter circle is here. Let me cancel out of the move copy for a second and it's very faint but if we have it turned on, even though that component is not active, we're in the rack component, you can see it right there and click on it. It's that dashed line here and we can see the diameter is 48 millimeters. Alright, so that tells us that we want to move down 48 millimeters because anytime you have two different gears, no matter the sizes, as long as you get that pitch diameter circle to be tangent, the gears will mesh. So again I'll pull up my move copy by right clicking, I'm going to change this move object to bodies, selection is going to be my body here and I'm going to choose the translate option, create copy, I'm going to make sure that's activated or enabled and I'm going to move this down, I can just go ahead and type it in right here at negative 48 millimeters and I'm going to click OK. Now I'm going to go back to that spur gear here, I'm going to activate that component and I'm just going to rotate this so that it looks correct. The important thing here is that this bottom gear that this tooth over here is going to be facing straight up, but just so that it looks right, I'm going to right click, go to move copy and I can rotate this by clicking on the body here, make sure I have body selected, my move type is going to be rotate access of rotation, I can select any one of these circles here, I'll go with that inner circle and now I can start moving this to give me a rotation. Now I can eyeball it, but you don't really want to do that, you want to be as precise as you can get, like I can see that that kind of works. So we want the exact number here and how do we figure that out? Let's back up for a minute and I'm going to explain this because to me, this is something I find really helpful, so I'm going to go under the assumption that you may find it helpful as well. Now you may be a math whiz but not all of us are and I am certainly not one of them, so I have to kind of think of the rational steps to slowly step my mind through how I can approach this and so that it makes sense versus just like, oh what's the formula do this because I find memorization to be useless. Okay, so the question I need to answer is what is the precise angle I need to move this? The great thing with Fusion 360, even if you're not kind of sure of the math, you can just figure it out by measuring. So let's go ahead and create a sketch. Now here I have the spur gear component activated and I'm going to create a sketch on that surface of that gear. So basically what I want to know, what's the angle to move this gear one tooth over? All right, so what I can do is project in two points. I'm going to hit P4 project, specified entities is selected and I'm going to click on two corresponding points on different teeth. So this point right here, if this tooth has moved all the way over one step it would be the same point here. I'm going to click okay and I'm going to draw a line from the center origin here to that first point and then draw another line to that second point and if I hit D for dimension I can click on both lines and I can see that that is 15 degrees. Perfect. That's all I needed there and the other way, if you just want to use math to do this, you can say well okay, if I take 360 degrees, which is a full rotation here and I divide it by the number of teeth that should get me that same angle, right? Because you take that angle times it by the number of teeth, you should get 360 degrees. So in that case we can do the math. I'll take 360 divided by 24, which will equal 15 degrees. So perfect. The math checks out. Wanted to show the two approaches there because sometimes we can just get overwhelmed by the numbers in the math but you know if you just kind of rationally step through it and just think of the problem and use the tools and fusion, you can work out the steps that you need to get there and it's okay and it's perfectly fine if you just have to kind of measure it first to understand it and then arrive at the whole, oh, it's just you know, 360 divided by a number of teeth. That's how my brain works. Okay, so I'm going to click finish, sketch here. Okay, now that I know the angle I need to rotate this, I'll right click, go to move copy. Again, move type is body, selection is going to be my gear, I'm going to choose the rotate option, select that inner circle and I can start twisting it. Now remember 15 degrees, if I do 15 degrees here, it's going to go one full rotation, which is really not going to help me. I have to take half of that to get it to go in between the two teeth there. So half of 15 is 7.5 and enter and there we have it. Okay, a valid question here would be what do I want a little clearance here between the teeth so they're not, you know, grinding? Yeah, you can do that. So instead of moving this 48, maybe I would move it down 48.2 millimeters, give me a slight clearance. But to be honest, I was curious and just tried printing it out with no clearance and it worked fine. The gears weren't getting stuck or grinding. So I'm just going to keep it as is here. But remember, you always have the option if you need to, to space that down a little more to give it a little more clearance and that would probably start with like 0.2 millimeters. Okay, I think I'm going to stop there for now. I can see that a full tutorial of the entire assembly is going to take quite a bit longer than I anticipated. So instead of making one really long video, I think I'll go ahead and break this down into a multi-part series. So next week we'll look at creating or jumping into that bottom gear there, that bottom spur gear. And we're going to isolate this one tooth here. It's the only one that's facing vertical, right? So we'll look at isolating it and creating a rectangular pattern of it so that we can create our rack here and also talk about the math involved to get the spacing just right. So stay tuned for that. I'll upload that video in a few days. In the meantime, if you enjoy this type of content, make sure to check out the additional resources I've linked below, including links to my online courses. I also do a weekly live Fusion 360 class that you can join. Or if you simply enjoy this type of content, consider becoming a Patreon member. All right guys, I will see you in a few.