 Hey guys, Vladimir here with Desktop Makes. I want to pick up where we left off, where we're looking to create this rack and pinion assembly here. So let's go ahead and jump right in. If you haven't seen the first video, just go ahead and check out my videos. It will be the one right before this one. Okay, so we created these two spur gears here. And the bottom one, we want to go ahead and take that and convert it into a rack. We'll go ahead and activate the rack components and I'm going to create a sketch on this bottom gear here. And what we're going to do is just project the outline of a single tooth. And now here it's important that this one tooth is facing completely vertical. So I'll hit P4 project and I have specified entities here selected. And I'm just going to click on the outline here. Just be careful, you do have to make sure you get the line. If you accidentally click on the inside, just click again to deselect it. And we're going to select these curves here. And then once you get your selection, go ahead and untaggle the body here. And you should see the outline there. That looks good. And then we're going to hit L for line and just connect these two bottom points. Now you can see here we have the purple outline, but it's not connecting because we can't get like a profile. This is what it should look like when we click on it. It should be highlighted blue. And I can tell if I zoom in here, I can see that it's because we have a gap here. Now a couple ways we can go about addressing this, we can just hit L for line and connecting these two lines. You know, you're perfectly fine just doing a line there. That length is 0.026 millimeters. So it's not going to affect it, especially since we're 3D printing this. But another way you can address it is just clicking on it, hitting delete. And then we can come in with a tangent arc. So under the create menu arc, we'll grab a tangent arc and then I can click on this top point and then click on the bottom. You can see it automatically adds the tangency and it will be good. Now if I hit D for dimension and inspect this arc, that's 1.028 and this one over here is a straight one. So it's not perfect, but again at the scale here we'll be fine. So in fact I'm just going to do the same thing for this one just so that they're both even. I'm going to go ahead and delete that and grab my tangent arc here and we'll go ahead and click on that top point and on that bottom point. Now you can see if I click on it, it highlights blue, so therefore I know it's a closed profile. So one important takeaway from here is when you do bring in geometry, either as an SVG or DXF or from projecting geometry and it doesn't highlight, you probably have an open connection there. And so zooming in to where these endpoints meet is a way to figure out where you need to address. Alright so we have what we need. I'm going to click finish, sketch here and then I'll hit E for extrude, grab my profile and I'm going to change the extent type to 2 object and I'm going to orbit to the back of the gear here, select it and it'll reference that as a distance. I'll click OK and there goes my 1 tooth there. I don't need to see the top spur gear there so I'm going to untoggle the visibility. And within my rack component here I can see I have 2 bodies, body 1 here which I don't need anymore. That was simply to reference that top tooth there to extrude it. So I'm going to right click on it and go down to remove. This will keep things a bit simpler. Okay now we're going to take this 1 tooth and do a pattern of it. So let me untoggle sketches, we'll go to a front view and now I'll grab my rectangular pattern tool under the create menu, go down to pattern, rectangular pattern tool. So here we're going to choose object type as bodies and we'll select our body. For our axis here we're going to select the bottom edge that tells it the direction we want to go and I'll just grab this arrow and start bringing it out. Now a couple important things we're going to want to do here is change the distribution type to spacing and the direction from 1 direction to symmetric. Now we have to figure out the distance and this is the distance between teeth here. So if we recall from the last video we had to figure out the angle between teeth on the circular spur gear and the way we did that is we took 360 degrees divided by the number of teeth and that gave us the angle between teeth. Similar type of concept here except instead of 360 degrees we need to take the circumference and divide it by the number of teeth. So if you consider that pitch diameter circle, if we take that let's say we cut it and we lay it out straight that would give us our circumference and if you remember back from your geometry days there's a formula for your circumference and that's 2 pi r. But if we write it in terms of diameter it's simply diameter times pi. So diameter times pi will give us our circumference and if we multiply that out it comes out to 150.796 and if we divide that by the number of teeth which we know is 24 that gives us a spacing of 6.283 between teeth. Now the cool thing with Fusion 360 is we don't have to type that number in here we can actually write it in terms of the formula so you can do the math directly in these dialogue boxes. So I'll start with a open parentheses there and I want to know my circumference and like I said that is going to be the diameter times pi. Now I know our diameter is 48 so I'll hit times pi you have to write that with capital P, capital I close parentheses and then we're going to take that and divide it by the number of teeth which is 24 teeth and there we go it's got our spacing right there and I'm going to increase the total number of teeth here the quantity to 21 and you should get something like that we'll click okay and we can measure that spacing right so if I go to inspect and go between this tooth here and the same point on the adjacent tooth I have it right there 6.283. Awesome all right now we are cooking so let's go ahead and continue the design of the rack I'm going to create a sketch and I'll just click on this first tooth here and I'm going to hit P4 project and I'm going to project that left point and the right point here click okay and then next we'll grab our three point rectangle tool here so the three point one is going to be useful here because we can simply click on the first point and then click on the second point here and then I'm just going to come down let me move to the right so we can actually see we're showing the distance there I'm going to type in three millimeters and hit enter okay if we're extrude we'll select that profile same idea here we're going to reference the back here to tell it how far to extrude so for distance we'll say two object and the object will be the back of any one of these two faces here make sure you're selecting the actual face operation is joined we'll click okay and now we have our rack here okay perfect so we're all set with the rack and we have our gear here if I toggle the top visibility of the parent component we can see them both here and so next there's one more thing we need to make which is just the base to you know put this whole thing together so that you know it can hold it in place and it can spin so to create the base we'll first have to create a new component right click new component here we're going to call this one base click okay and we'll create a sketch on this midplane here so that green blue plane if you're having trouble selecting it just untaggle the visibility of that spur gear and go ahead and click on it and okay we're going to bring that gear back on so we can see it and we're just going to move the view cube here so we're looking at you know this orientation and my screen it's going to be the left view here with the left written downwards all right so here we're going to project a few points here so p for project actually we'll do a couple lines and a point so we're going to do this line here the bottom and then we're going to project just the top point here of our gear so we're bringing those points into this current sketch we'll click okay and now we should see these purple lines and points we're going to reference those to create an outline here so l for line in here i'm not going to worry so much about distance or whether my lines are straight so i can just kind of do something like this you know just being sort of purposely sloppy here just to kind of speed things up but it doesn't matter because we're going to come back down and close it here and then we'll add some constraints to make it exactly what we want so you should have something like this we basically are just drawing sort of an l shape around these points here and i'll go ahead and grab my horizontal slash vertical constraint and i'm just going to click it on each one of these lines to make sure they're either vertical or horizontal and i'll just click on all of them if they're already vertical for example just give you an error but that's fine okay next we're going to add some dimensions so d for dimensions i'm going to click on this top edge here and i'm going to make that five millimeters and now i'm going to keep adding dimensions and i'm going to continue to reference that dimension the first one by clicking on it and you see here it'll say d 55 years will probably have a different number but as long as it's saying d and referencing that first dimension you're good and the reason i'm doing this is because if i want to come back and change that thickness here all i have to do is change that first one so let's say i wanted to do seven you'll see that they'll all update and i don't have to worry about changing each one of them okay one more dimension just this line here i'm going to make this 65 and there we have it i'm going to click finish sketch click on this profile here e4 extrude in here i'm going to go with a symmetric extrusion and i'm just going to pull this out until it extends past the rack here so let's say we'll enter a distance here 70 looks good okay and there we have it i can untie all that sketch there i don't need to see it and there is our base so if we activate the parent components here the whole assembly we should have something like this okay almost there just a few more things we need to do i'm going to go back into that base components and i want to go ahead and create the sort of pin here to come out for the spur gear to be able to rotate about so let's go ahead and create that and so we're in the base component here and i'm going to create a sketch on the back here and i'm going to orbit back to the front and i'm going to project this circle here so p for project i'm just going to grab it click okay and if i go to the back i should see it all right we'll go ahead and untie all bodies there just so we can see the circle a little better and i'm going to untie the rack and spur gear components and for sketches i just need to see the second sketch here not both of them all right here we're going to come in and do an offset and i'm going to click on the circle here and i'm going to do five millimeter offset and then finish sketch okay i'm going to bring that sketch back into view and let's also look at the body there because we're going to select these two circles in extrude immense so if we're extrude click both of these circles and i'm going to go inwards a distance of negative three millimeters operation is going to be new body and then i'll click okay and if i untangle the top of body here i should see that i should just have this disc here i'm going to click on that second circle if we're extrude again this time i'm going to bring in body one and i also want to see that spur gear because what i want to do is extrude this out and have it go past the gear in here negative 20 millimeters looks good now i want to have this be a join but i don't want it to join the back portion here of that base so let's untangle body one and i should just have this here in fact it's not going to go ahead and join into the spur gear because that component is not activated so i don't need to untangle the visibility of it but we don't really need to see it anymore i just want to reference it now we can just go ahead and untangle it and we should have something like this i'm going to click okay and there we have it that's our pen let's bring back body one of the base component here and we'll untangle sketches and we can see now if i untangle between this and this body we've got two bodies there and they overlap each other now i want to use the pin here to cut out an opening for it on the base so to do that we're going to go to modify combine and our target body is going to be the base here the tool body is the pin operation is cut and we want to make sure keep tools is checked because we want to keep our pin click okay and now if i untangle the pin there you should see we have the hole there and the idea is to be able to just kind of snap the pin in there everything looks pretty good here one final thing we'll need to do is factor in how everything is going to fit together and so we're going to have to design a little bit of clearance fit here and so to do that consider our rack sliding back and forth here we're going to need to give it a little spacing otherwise it's just going to bind or probably won't even fit so let's start with that i'm going to go ahead and grab my offset face tool here under the modify menu i'm going to click this surface here on the back and on the front so two opposite surface and i'm going to go a distance of negative 0.2 millimeters now this is something you may need to experiment with or just know your printer i'm going to go with 0.2 because i think it'll be good enough for my printer you may have to do a 0.3 millimeter clearance there if you find that you still need a little more room there but i'm going to go with 0.2 click okay and the next clearance i'm going to want to put in here is on the opening here for our pin to fit in here and again we'll go to modify offset face i'm going to select these two surfaces here and i want this one to be more of a friction fit so i'm going to do negative 0.1 and click okay or enter and there we have it now if i bring that body into view i can see if i go here and zoom in there should be a little gap in between there which is exactly what i want so let's go ahead and activate the top level of the component and bring both all components into view and there we have it here so if i zoom in here i can see a little spacing between the front and the back and of course the spacing between the pin there okay so that's how we create this rack and pinion assembly with the spur gear our rack and we have our base i'm going to end it right here in the next video i'll show you how we can add motion to our components by applying joints and also a motion link so stay tuned for that video all right if you have any questions or comments leave them below also check out the links below to my fusion 360 resources i've got courses a weekly life class that i offer or if you simply want to support me creating more content like this consider visiting my patreon page and supporting my channel all right guys i will see you in a few