Build a Lego Helicopter in SolidWorks 3D CAD

1. Welcome to the Course: Hello and welcome to this SolidWorks project-based course on how to make a Lego helicopter like this. This course is mostly designed for people who already have a little bit of SolidWorks knowledge. But now I want to practice those skills in a fun way. My name is John Olson and I'm a design engineer and product designer, and I've been using SolidWorks since 2006. I previously created a range of SolidWorks courses that take people from being complete beginners all the way up to being competent users. But for this one, I wanted to do something a little bit different. During the course, we'll create a complete Lego helicopter assembly, will build every single part from scratch. We'll put them together and then we'll even add mechanical mates that allow the blades and the tail rotor to spin around like this. The course isn't really designed for complete beginners. It's more for people who know a little bit about SolidWorks who are maybe a little bit rusty and want to practice. Having said that, if you are completely new, then we do start off fairly slow and then speed up as we go through. So feel free to give it a try and just follow along the videos. And if you do get stuck anywhere, then just send me a message and I'll try to help you out. With that in mind. Let's get started making our Lego helicopter. 2. How to Use This Course: Before we actually start building the Lego parts, we're just going to have a very quick video that explains the best way to get the most out of this course and how to use it. To use this course, you'll need your own copy of SolidWorks. The course is recorded using SolidWorks 2021. But if you're using a different version, then you can still use the course. All the versions are very similar. You might just see some very small differences in things like how the interface looks or minor tool options. If you do run into any problems, then please just send me a message. This course does how exercise files that you can download and use. These are the PDF of the helicopter instructions and a SolidWorks model of the finished chopper. You don't actually need these files to complete the course. They're just a bit of extra information if you get stuck on apart and you want to have a look at it in 3D. Now, solid works files aren't backwards compatible. These files have been made in SolidWorks 2021. So this means that you will only be able to open them if you're using 2021 or newer. For example, SolidWorks 2020 or earlier, weren't open these files. However, the exercise files also contain a finished version of the helicopter saved us a step file. This will work with older versions of SolidWorks. You just won't be able to edit all of the parts like you would with normal SolidWorks part. But you will still be able to see it in 3D and measure it and spin it around and so on. To use that step file, just drag it into SolidWorks and it should open. Those exercise files can be found for download under the projects and resources tab. This course does assume that you have a little bit of SolidWorks knowledge and you know how to do things like making features and sketch it. It's designed more for practicing SolidWorks skills than learning completely from scratch. Having said that though, it does start off fairly slow. So if you're totally new to SolidWorks, then you can try just following along. You can also slow down the video speed using the controls on the player. If you do get stuck anywhere, then feel free to send me a message or ask a question using the Q&A feature below. And I'll try to get back to you as soon as I can. Before asking a question. It might also just be worth quickly searching the previous answers or searching online to see if it's already been answered. That might just get you a little bit of a faster response if I'm not on my computer. If you do want to get the Lego kit yourself and have a go at measuring it all and making it yourself. Then the serial number of a is 30465. It cost me about eight pounds, which is about ten or 11 US dollars, I believe. Then just warned final note, this course is taught using metric, using millimeters. If you prefer to use something like inches or a different set of units, that's absolutely fine. You can either change your units to millimeters or when you're using the smart dimension tool, you can input the millimeter values that are used on screen. But before you press Enter, you can type in MM for millimeter. This will then convert the millimeters to inches or whatever kind of units you are using. With all that out of the way, let's jump in and start making the first parts of our helicopter. 3. Creating the Axle: To create the Lego helicopter, we're going to go through and follow the Lego instructions like you would if you were making the lego model in real life, the kit comes with 70 pieces, but there's actually any 31 unique parts because some of them are used more than once over those 31. Some of them are very similar to each other. So we don't really have to make 31 completely different parts. Starting with step one here, we've got four different parts to make this first stage. We're going to make those parts one-by-one. And we're gonna start with probably the simplest one, the axial here. If we look at the instructions, we can see there's a number three next to the axial, and that indicates the length of it. That means that it's actually three bricks long. If we put it inside the brakes like this, you can see it goes through three sets of Brex. We're going to open up SolidWorks and start to create this part. Want SolidWorks is open for you. Just start a new part. So here we are in a completely blank part. When we start a new Solid Works part, we usually start on one of these three default planes, the front plane, the top plane, or the right plane. Now sometimes when you look at the items you're making in SolidWorks, there'll be a really obvious top or side or front of the part. And you can line those up with the planes in SolidWorks. But actually in the case of this part of the Lego axial, it doesn't really matter too much. Which direction is the front, the top, or the side? In this part don't get too hung up on which plane you should start on. In this case, I'm going to start on the front plane, so I'm going to left-click to select that plane. And then I'm going to choose sketch from the pop-up menu, which will start a new sketch. Now we've moved to a normal to view and we're sketching on the front plane. The first thing that I'm gonna do is draw that cross shape, which is a cross-section of the axle. To do this, I'm going to draw two rectangles. So I'm gonna go to the Sketch tab, choose the rectangle tool, and we want to choose a sensor rectangle, which is the second option here. You can click on the little drop-down and you can choose center rectangle directly up there on the command manager. Or you can just choose the tool and you can choose center rectangle here on the left. So if we look at the little icon in the tool, you can see there's two numbers. Number one indicates the first click. The first click sets the center of the rectangle, and then number two indicates a second click that sets the overall size of the rectangle. I'm going to move into the graphics area. I'm going to start at the origin, and I'm going to left-click once at the origin to set the center of the rectangle and then move the mouse out. Then I'm going to click again to set the size of the rectangle. We want something like this. And then remaining in the sensor rectangle tool, I'm going to go back to the origin and I'm going to draw another rectangle, but this time in this sort of direction. This one should also be linked to the origin. And then I'm going to press the Escape key just to close the rectangle tool. Now when you drawing his sketches, it's a good idea to always try to link them to a fixed point, which in this case is the origin. This then allows you to fully define your sketches so they won't move around or change shape or size when you don't want them to. Now that we have our two rectangles, we're going to use the smart dimension tool to set the size of them. Jews, the smart dimension tool from the command manager. And then I'm gonna set the size of this rectangle at the top here. You can see when I choose that line is coming up on my view as 36 millimeters. But I'm gonna change that to 1.8 millimeters, which is what I've measured from the axial using my digital calipers. Now you can see when I had that first I mentioned the whole sketch has resized automatically. This only happens when you add the first dimension of the sketch. Then for the height here, I'm going to choose this line by left clicking, and I'm gonna make that 4.7 millimeters. Now we want to make the second rectangle the same size as the first. We could add some more dimensions, but instead we're going to use relations. I'm going to press Escape to close the Smart Dimension tool. What we're going to do is select this small line that we've already mentioned. Left-click on it to select it, and then hold down the Control key. This allows you to select multiple items. Then we're also going to select the second line here. Now I'm going to release the Control key. And you can see we get this pop-up menu with different relations on it. From the pop-up, I'm going to choose this one which is make equal. You can also choose it here on the left is exactly the same setting. By clicking that it means that both of those lines are now an equal length. They're both the same size. And if we click on one of those lines, we can now see we've got the equal symbol on both of the lines. Then we're going to do the same thing with a longer line. I'm going to select the one that we've already mentioned, hold down Control and then select the second one and then release control. And then from the menu that pops up, Let's choose make equal. Those lines are now the same site and you'll notice that the entire sketch has turned black. This means that it's fully defined. We also have a message down here that says the sketch is fully defined. This is because both of these rectangles are fixed to the origin so they can't move in position. Then we've set the size of both of them as well so they can't change in size. We could now extrude this cross-shaped profile to make our axial shape. But actually if we look really closely at the axle and we looked at it from the end, we can see that these edge faces aren't actually completely square. They're slightly rounded. This is so that we can put the axle into a round hole and it will still spend around properly. If we actually look at that part, it's going to be really hard to measure that radius. But what we do know is that the widest length across the axial is 4.7. What we can do is get the circle tool from the sketch tab. Then let's draw a circle. Let's fix at the origin and drag it out to about this size. Then press the Escape key to close the circle tool. We can then left-click to select that circle. Hold down control, which allows you to select multiple items. Then we can select one of these small straight lines, then release control. And from the menu that pops up, Let's choose make tangent. Now that circle is exactly touching that small straight line. That will just give us that slight radius that we have that that lets the axle spin properly in the hole. Now we have everything we need in terms of our sketch and we can extrude this profile to create the axle. We can stay within the sketch. We don't have to exit. But let's go to the Features tab and let's choose extruded boss base, the first option here. We can now say that we don't get any kind of preview for the extrude. And that's because we've got these overlapping profiles within the sketch. So SolidWorks doesn't really know which areas of the sketch we want to extrude. So we have to choose those manually. And you can actually see if I hover over these different enclosed areas in the profile, they turn red. And that indicates that we can select those areas. Let's select all the areas we want to extrude. There's four outer areas of the cross shape and then there's that center section as well. Now we can see there on the preview we've got that cross shape, but the edges of the crosscut a slightly curved. If you're having any trouble selecting those areas, you might just have to click down here in the selected contours box here on the left, and then choose those five different areas. So we've got that center section and then we've got those four sections around the outside. Now we can extrude this actual shape, the exact length that we want. But before we do set the length, I'm gonna change the end condition from blind to mid-plane. This means that instead of extruding and just one single direction, we're gonna be extruding in two directions from the sketch by an equal amount. Then we can set the exact length and we know from measuring it with the calipers that that's 23.45 millimeters. And we can see on the preview that we're gonna be extruding equally in each direction. When you happy with that, you can press Okay to create that feature. Now we've created that basic actual shape. Now if we look at the axial part in real life very closely, there's actually a lot more detail than we can see here on the model. We've got some parting lines on there from where the mold moved apart, we've got some ejector pin marks from probably where the part was pushed out of the mold. And sometimes you've even got small part numbers and things like that. In this case, we've got some slightly rounded edges to help you put the power into the other bricks. It's really up to you how much detail you want to model at this stage. This really is a trade-off between how much time you want to spend and how accurate you want your parts to be. I would personally say that we don't actually need all of that super fine detail. But what we will do instead is just round off the edges of the axon here. Let's select the fillet tool from the Features tab. And I'm going to make a filler that's nought 0.5 millimeters in size. It's just symmetric, a circular profile. And I'm going to select these four edges around here. There's four on this end, and then there's another four. On the other hand, if you find that you accidentally select the wrong face or edge, you can just click it again to de-select it. Again to add those four fillets on each end, 18 total, and then press Okay. Now we've got our basic axon model there, and that's all there is to this first part. We can now save the part. And you can do this by pressing Control S. You can press the Save icon or you can get a file save. I'm gonna go to my working folder where I'm going to put all these different Lego parts. And I'm gonna call this part something descriptive like axial. Now before you press okay, whenever we're saving parts in SolidWorks, try to avoid quite generic names, things like block or axial or connector. That's because if you create a similar project in future, may be sitting there isn't lego, but something that also uses an axial, then it might cause problems to your assembly. If you've got multiple parts named the same thing in different locations, you might end up using the wrong part in your new assembly. To try to avoid this, I'd recommend adding some kind of unique identifier to your paths. It could be just something like the date or it could be a part number. You can maybe even write something like Lego chopper axon. But what I'm gonna do is write axial. Then I'm just going to add on 30465, which is just the model number of these like Okay, I'm going to add that number to all of my parts just to make them unique to this project. I'm gonna say axial 30465 and I'm gonna save that part. That's all there is to that first part. So we've got one down 30 to go back. Actually, some of the later ones are very similar to these early ones. So we can just copy and paste them and make some small changes. So it's a very quickly recap this part we just made a simple extrude using that cross shape with the rounded edges, and then we fill it at the edges there. In the next video, we'll start making the next part, which is not right angle being, which makes up the side of the fuser larger the body of the helicopter. 4. Making the Right Angle Beam - Part 1: Welcome back. In this video, we're going to make the second lego part, which is the right angle beam, to start off open SolidWorks and open a new part. As before with the first part, it doesn't really matter which plane you start on. In this case, I'm gonna start on the front plane again. So choose the front plane and then select sketch from the menu that pops up. Now if we look at the beam part, we can see it's basically made out three rectangles. They're at different angles to each other and the ends of those around it. So we can use the slot tool to draw this basic shape from within your sketch. Let's go up to the sketch tab and choose the slot tool. And we want to choose the first option, which is a straight slot. We can see on the tool as usual, you've got these little numbers on the icon and they show you what each click does within the tool. Number one sets the left-hand side of the slot. Number two, since the right-hand side. And then number three sets the size of the slot. Let's go into the graphics area and start at the origin with the first click. And then let's draw our slot, the goat to the right horizontally, something roughly like this. That's going to be the bottom of our beam. We're now still within the slot tool. And let's start another slot at the center of this right-hand point, going upwards and to the right at an angle. It doesn't have to be exactly the correct angle because we will add dimensions in a moment. We'll go upwards, something roughly like this, and then finish that slot there. Then let's start a third and final slot that starts from the center point on the right here and goes directly upwards, vertically. So you should have something like this and then we can press escape to close this lot tool. Now the first thing that we're going to do is just select all three of these slots and make sure they're all the same diameter. So let's select the rounded edge of each slot in turn. So I'm gonna select this one on the left. You're going to hold down Control and then select this one in the middle. And then keeping control held down, select this one on the right, and then release control. And then from the menu that pops up, I'm going to choose make equal. That will make the radius of all of these three slots the same. Now we have a rough overall shape of the beam and we can start to set the exact size. So let's choose the smart dimension tool from the sketch tab. And the height of that slot from what we've measured with the calipers, we know is 7.4 millimeters. So when we add that first dimension, it resizes the entire sketch to suit that dimension. Next, we want to set the length of the bottom of this beam. And to do this, we're going to count how many circles are in that bottom section. So if you look closely at the partner is actually seven different circles in there. We also know from measuring the circles that they're each eight millimeters apart. And we know that the diameter of them is 4.8 millimeters. I'm going to get the circle tool from the sketch tab. And I'm going to draw a circle here on the left-hand side of our part is lined up with the origin, which means it's also concentric with that curved part of the end of the slot. Then I'm going to use the smart dimension tool to set the diameter here to 4.8. So we've got the first circle that we need there on the left. We know that the seven of those, and they're spaced eight millimeters apart, we can pattern some more of those circles along to set the exact size of this beam. Press Escape to make sure you're not in the smart dimension tool still. And then left-click to select that circle. Then I'm going to go to linear sketch pattern, which is on the sketch tab. We can now pass in this circle along. So we know we need seven instances. So I'm going to increase the number of instances to seven. And we also know that the spacing is eight millimeters, so I'm going to set that here as eight millimeters. Now if you don't see a yellow preview like this, just make sure you have that circle selected in the entities to pass inbox. And then make sure you also have a direction selected in direction one, you might just need to click in that box and choose one of the straight lines going in the x-direction. Now one last thing we need to do before we press okay, just put a checking this box that says dimension x spacing. This will just mean that the eight millimeter spacing will be set when we create the pattern. Then when everything looks good, press Okay to make that pattern. Now we can see we've got seven of those circles and we've got the eight millimeter spacing there. So all of those circles are black because they're fully defined. What we can do now is grab this end point of the lowest slot. You might have to zoom in a bit to be able to see it. So grab that and left-click and drag it. So it's lined up with that right-hand circle. The circular edge on the right-hand side of that bottom slot should be concentric with that right-hand circle. So what you can do is just drag that sensor point of the slot along and then hover over the edge of that right-hand circle. And then you should be able to see the center point of the circle. You can then move the sensor point in this slot back to the center point of the circle and release it, and that should link it there. Now we know that that lower beam is the correct length. Next, we can move these other sections around a bit. Firstly, let's just move this down a bit. And then let's get the smart dimension tool and let's add an angle in there. This is a 135 degrees. Now we can set the length of these two extra slot. Again, let's select the circle tool. And we know that this vertical section has got three holes in it. So use the circle tool to draw one circle here at the top, another circle here at the bottom of the vertical section. And then a third circle in the middle of that vertical section. So it should be coincident with the midpoint of that center line that goes down the middle of the slot. Then we can select all three of those circles. So remember hold down Control to select multiple items. Then just left-click to select those three circles. Then keeping control held down, let's also select one of those other circles that we've already defined. Then release control and just choose make equal. That will make those three circles on the right-hand side the same diameter as all of the other circles. We can then just set the distance between the holes. So use the smart dimension tool and choose, for example, the top one and the sensor on and set that to eight millimeters, that standard distance there. Then the final thing we need to do is just add that slot in the middle of that diagnosed section. To do this, we'll use the slot tool again. Choose the tool this time instead of a straight slot, we're going to use a sensor points lot. That's the second option here. So this means that we're going to start from the center of this law. We're going to move outwards and then set the size. And if we look at the numbers on the icon, we can see number one, the first click sets the center point of this law. So let's zoom in a little bit. Let's start the slot from the center point of that diagonal section. And then we're going to drag the slot upwards, something like this. Set a rough length of the slot and then drag it outwards and then set a rough size. Then once you've got the slot in place, press Escape to close the slot tool, and then we can make sure the slot is the same diameter as those other circles. So select one of the circles, hold down control, and also select one of the circular edges of this slot and then choose make equal. We know that slots to the correct size, but we can still move it around. If you're ever not sure why selling steel blue, why it isn't fully defined. You can just left-click and drag the points around. And that should give you an idea of what it needs to be fully defined. In this case, we need to use the smart dimension tool and we need to set the correct spacing for the length of that slot. So that length there should be eight millimeters. So that double slot is basically two holes that are joined together. Again, we're still not quite fully defined. So if I grab one of the points and move it around, you can see we just need to set the distance from the corner of that beam to the slot. That should be eight millimeters, because the space in-between all of the holes is eight millimeters and that should fully define your sketch there. And if you find you're not fully defined, you might just need to add some further spacing between the holes to make sure all of the holes are eight millimeters apart. And then the size of all of the holes should be 4.8 millimeters diameter. That gives us the overall profile that we need to create that bean shape. And we can now use that to create an extrude of the beam. So staying within the sketch, let's go to the Features tab. Let's choose extruded boss base. And then first let's set the width of this beam so we know that 7.85 us change it from blind to mid-plane. There are playing is down the middle of the beam. This will just make things easier when we need to mirror some features later on. Then let's click in the selected contours box and let's choose the areas of the profile that we want to extrude. So we're just going to select those gaps in the beam area. So it looks something like this. And as well as that main beam shape, we also want to choose the last and the first circle. That's because if we look at the real part, these first, unless circles are actually cross-shaped so they can fit in the axial part. So we're going to cut those separately. Then press okay, and now we've created the start of our beam there. So you should have a shape, something like this. Let's rename that first feature on the left by doing a slow double-click on it or selecting and pressing F2. And I'm going to call that beam. Now if you've seen any of my other videos, you've probably seen that I like to rename a lot of features. You don't have to do this. They can save you a lot of time in the long run just by making a model a little bit more organized and easy to understand. Now that we've made the basic beam shape, we're going to cut those cross-sections out where the axons will fit in. I'm going to start another sketch on the front plane. Let's start with the left-hand one down here. Firstly, get the circle tool. Draw a circle at the origin. So it's concentric without rounded edge of the end of the beam. This circle is the same diameter as the other. So use the smart dimension to set that as 4.8 millimeters. But we also know that he's got that cross shaped to fit the excellent. Let's go to the rectangle tool. Let's choose the center rectangle, and then let's draw two rectangles that make a rough cross shaped like this. And then use Smart Dimension to set the width of one of those rectangles as 1.8. We can now use relations to fully define the rest of the sketch. Firstly, I'm going to select the small edge of one of those rectangles and then hold down control and select the other small edge. And then make those the same length. So press make equal. So they should both be 1.8 millimeters. Then next let's select one of those small lines. And then also select the circle and make those tangent. And then do the same for the other rectangle as well. At this point, you should have that cross shape with a slightly rounded edges. And it's basically the same profile that we use to create the axial in the last video. Now if we look at the real part, there's actually also another area cut out here to the right-hand side. To create this cutout area. First, we're going to select that circular edge on the second circle there. And then go to the Sketch tab and choose Offset entities. We want to offset 1.3 millimeters outwards. You circle should be exactly touching the edge of the beam that if you find that your yellow preview circle is smaller than the IgE you selected, you might just need to press reverse here on the left. Then press Okay to offset that circular edge. Then we're also gonna do the exact same thing for the first circle we drew. So select that circle on the left, go to the Offset Entities tool and then Offset 1.3 millimeters outwards. The next we're going to select this upper straight edge of the beam. We're going to offset that one millimeter downwards. We're gonna do the same for the bottom edge of the beam. So select that straight edge on the bottom and then offset this one millimeter upwards. So we're building up a profile that we're going to cut out. Then finally, we just need to fill in a little gap here. So let's choose the Line tool and let's add a small straight line going from the edge of this rectangle out to that circle there. And then the same on the bottom as well. This looks like a fairly messy sketch, but we're gonna cut out specific parts of it. And this will become more clear in a moment when we actually make the cup. Before we actually do make that cut, we need to make the same sketch on the right-hand side for that final circle as well. So zoom out and basically follow the same process for this area on the right-hand side. We're gonna do this one a little bit more quickly. First I'm gonna get the circle tool. We're going to draw a circle which is concentric with the end of the beam here and set that to 4.8 diameter. Then I'm going to use the sensor rectangle to create those to censor rectangles. I'm going to set the size is 1.8. I'm going to make both small edges of the rectangle the same size by using the equal a relation. And then I'm going to set the length of the rectangle by making those small edges tangent with the edge of the circle. Then if you remember, we use the Offset Entities tool to offset those circles 1.3 millimeters, you might need to choose them both separately and do two separate offsets. You might be able to choose them both and then do the offsets in one single go. Then again, we're going to select those straight edges on the outside of the beam and offset those worn millimeters inwards, one on each side. Then finally, just use the line tool to add those two small lines to join that small cross part. The rest of the cutout. We're now ready to make those cutouts from still within the sketch. Let us go to the Features tab and let's choose extruded cut. And then click down here in the selected contours box. We want to choose these five sections of the cross. We also want to choose the extra small rectangle section and then also that kind of wedge-shaped section there. Then for the type of code instead of blind, Let's go for through all both. This just means that you cut through the entire model in both directions. If we now zoom in and look at the preview, you can see we've got two small areas that we also need to cut. We also need to select these two small wedge-shaped sections, one on each side. And then when you've got everything, it should sort of look a bit like this, sort of like a gravestone on a half-pipe almost. Then let's go to the other side and do the exact same thing. We're going to choose these five sections of the cross. That wedge-shaped part, the small rectangle, and then those two small wedges. When you're happy press Okay, and it should look something like this. We've cut out the area for the axial on both sides and I'm just going to rename that feature as axial cut. The general shape of the part is complete there. If you stopping at this point, you can save your partner. I called mine corner beam seven by four by three, just because it's seven long by four by three. Then I put that number on for the kit which is 30465. If you're not stopping, you can just continue directly onto the next video where we'll just finish off some small details of this part. 5. Making the Right Angle Beam - Part 2: In the previous video, we started to create that right-hand beam. Now this is one of the more complicated parts, so it's a little bit drawn out, but we can actually repurpose this part to create a few of the other beam parts later on, and that should save us some time. So continuing on from that previous video, we've got the basic beam shape. In this video, we're going to add the final finishing details for the first set of details that we looked at the beam closely and we looked at the holes. You can see they've actually got a wide hole around them, which only goes in a small distance. To create this, we're going to start a sketch on the side face of the beam. So select the face of the beam by left clicking. And then from the menu that pops up, choose sketch, then select the edge of all of the circles. Remember you need to hold down Control to select multiple items. We also want to select the slot here. You'll need to select the four different elements of it separately. So there's two curved edges and then there's two straight lines connecting them. Now we want to offset these edges so we can make that slightly larger cut. But sometimes you'll find with the Offset Entities tool when you select the tool and try to offset, sometimes it doesn't seem to work like this. If this happens to disclose the Offset Entities tool, we've still got all of those edges selected. And then instead of offset choose convert entities, we've now converted all of those edges into new sketch entities. We can then select all of those sketch entities. You can do this by pressing Control a, which is select all or you can just drag a box around all of them. And now we can offset those converted edges. So sometimes if you select an edge directly and try and offset it, it won't work if you convert it first and then offset that converted line, it will work. We're going to offset 0.7 millimeters. And then before you press OK, here in the construction geometry options, we want the offset geometry to be solid, so there shouldn't be a check mark in that box. But we can actually make the base geometry into construction geometry. If we put a check in that box when we press Okay, it means those original baseline that we selected will be turned into construction lines. Let's press Okay, and if we zoom in a little bit, we can see there's original selected lines are now construction lines for the offset lines are solid. We can now do an extruded cut. And we've measured the depth of that car as 1.25. Now, just a very quick aside to measure the depth of holes like this using your digital calipers, what you can do is just open the jaws of the caliper like you're going to measure something. And then if you look at the end here, there's actually little tablet sticks out at the bottom. You can use this to measure the depth of things. After making that cut feature, I'm going to rename it as whole surround. The next thing that we're going to do is cut out the small cavities between the circles. Start another sketch on this face. And first we need to offset all of these circular lines. So again, let's select the edge of those larger circles. And we're also going to select the edge of this law. Now with the slot, instead of selecting each element individually, you can also just right-click on one of them and choose, select tangency. And that will select all the lines connected to the one that you right-clicked on. Then I'm going to offset those edges. And again, if you find the offset doesn't work, remember that you can first convert those edges, and then you can select all of those converted edges by pressing Control a. And then you can offset those converted lines. Then let's offset 0.55 millimeters. And again, we want to make the baselines construction and we want to make the offset lines solid. So now we have all of those lines, they're larger than the circles in the slot. Next, we just need to offset the edges inwards so that we can cut out the correct area. I'm going to select each straight edge in turn and offset it inwards one millimeter. Then let's do the same for the upper one here. Then the same with the diagonal one here. And also on the other side. Then finally just the short vertical one here. And also on the other side. Now we can cut away those cavity areas between the holes by using an extruded cut which is on the Features tab. This current is three millimeters deep, It's blind. And then in the selected contours, Let's just choose all of those. So of our glass shapes that are between the holes should have all of those wounds between the circles and the slots like that. And then press Okay to create those. And let's rename that feature as cavity cut. We're almost done now one of the final things we'll do is just get the fillet tool. Let's choose a 0.5 millimeter filler, just a round fillet symmetric. And let's round off the inside edges of those cavities. We want to select these four edges which are in-between each set of holes. He can select them manually. You should also find that when you select one you get this edge selection toolbar pop-up. This will give you different options to select multiple edges at the same time. I'll show you again with this cavity. When you select the first edge, we get this puppet toolbar. And then if we just hover over for me, it's that first option that will allow me to select all four edges within that cavity. That just saves a little bit of time. So I'm gonna do the same thing for all of these cavities that are between the holes. So as we go around, there are other options on the Edge Selection toolbar. Most of those aren't really relevant to us. Let's just try and stick with that first one. For each set of cavities, we can choose four edges at the same time. It might take a little bit of time to select these. You might need to spend your model around a little bit as we go around the corner to help you select the correct edges. And if you find that you select the wrong face or the edge, just click on it again to de-select it. When you've got all of them, it should look something like this. We've got all of those internal corners there. But we're going to leave the ones on the edge here for now because we're going to mirror these fillets over. And if we mirrored those, it would cause a problem because they actually go all the way through press Okay, to create those fillets. And it should look something like this. We've got all of the detail that we need on this first slide, but we don't have any of it on the opposite side. But because we used a mid-plane extrude, we can actually just mirror everything over. So let's select the front plane by left clicking. Then that's also hold down control and select those three latest features. It's the whole surround, the cavity cut and the fillet. We should have three items selected as well as the front plane. Then we can press mirror and we can see we get a yellow preview like this for the mirror plane, we've got that front plane that we selected. And then for the features to mirror, we've got the whole surround, the cavity cut and the fill it. If you find that your preview or you mirror it doesn't work, try going back into that first feature and just making sure that you've got a mid-plane extrude there instead of a blind extrude, that just makes sure that the front plane is at the middle of the model. So we can use it to mirror these items over. Press OK. And now we can see that we've mirrored those features over onto the other side. Then the final thing that we need to do to finish off is just use the fillet tool again, keep the same settings. So 0.5 size, it's a symmetric round fillet. We're just gonna get these four edges here on the left. And the reason that we didn't add these to the previous fillet before we did the mirror is because these visits actually go all the way through. We can't actually mirror them through if they're already all the way through. Then going up here to the top, there's another four on this side. So there should be a edges in total. And then press Okay to create that fillet feature. Now we have created that being part. And the final thing I'm gonna do is just change the color of it so it suits the color in the instructions. You don't have to do this just might make it a little bit easier to follow the instructions if all of the parts on screen match with the parts in real life. I'm going to open the Appearance scenes and Details tab here on the right. I'm going to choose appearances. And then here in appearances I'm going to choose something like a plastic medium gloss, and I'm going to go white color. And then double-clicking on that color applies that appearance to the whole part. Then the final thing to do is just save the part if you didn't already save it in the previous video. As we mentioned before, I'm gonna save this one as corner beam seven by four by three because there's seven holes along the bottom. There's four at that diagonal corner because you remember that slot counts as two holes and then this three on that vertical section. And then also I'm just going to put that reference number on the end, 30465. And then we have our finished second part. In the next video, we're gonna do something a little bit simpler. We're going to make that friction pen parts. 6. Building the Friction Pin: The next part that we're going to make is a very small part of it is used quite a lot in lego. Will be able to use it multiple times, and that is the friction pen. This is often used to connect different parts together in SolidWorks, let's start a new part. And this time I'm going to start sketch on the right plane because I'm actually going to start from the middle of the part and then we're going to model it outwards in both directions. I'm going to start sketch the circle tool, and I'm going to draw two concentric circles fixed to the origin. These are going to be that wider ring at the center of the connector. I know that the inner diameter is 3.5 millimeters. We know that the outer diameter is 5.85, so we'll add both of those dimensions that should fully define the sketch. And we can then do an extruded boss base mid-plane. The thickness of this is 1.6 millimeters. We're going 0.8 in each direction, 1.6 in total. This is that thicker section at the very middle of the connector. I'm going to rename that feature as something like middle ring. Next up, I'm going to start another sketch also on the right plane. I'm going to use the inner circle so we can get the same inner diameter. I'm going to select that circular edge and then press convert entities. So now we've got that circle in our sketch. Then I'm going to get the circle tool again. I'm going to start at the origin. If I go to a normal two view, you can see a bit more clearly. This circle is a little bit smaller than that first one. For the size of this is actually 4.7 millimeters diameter. Then we're going to do another mid-plane extrude. So we're gonna get Features extruded boss base going to set it to mid-plane. And this warrant is 14.7 millimeters in size. So now we have that wider section in the middle, we've got the same boar or inner diameter all the way through. And then we've got that smallest section that goes out to each side. I'm going to call that second feature something like out-of-body. The next thing that we've got is a small rim right on the edge here. I'm gonna start a sketch on the outside face. I'm going to select that inner diameter and convert it using convert entities. Then I'm going to get the circle tool, start another circle which is concentric with that one. This one is a little bit larger than that widest section, but it's not quite as large as that middle section. The size of it is 5.25 millimeters. Then we can just do a blind extrude outwards 0.5 millimeters. Only sticks out a really small amount like that, just off the end. We've still got that same inner diameter all the way through and I'm going to rename that new feature as outer rim. It's exactly the same on the other side so we can mirror that outer rim feature over. I'm going to select the outer in feature. I'm going to also select the right plane. And then I'm going to press mirror. We have the right plane here as the mirror plane. Then we've got the features to mirror as the outer rim and then press Okay. And that rim is also added to the other side. There's a lot of extra detail on this part that we don't necessarily need to add for the SolidWorks model, there's some really tiny numbers which are probably the part number. There's some little extra ribs that may be give it a bit more friction in the hole. And there's even some ejector pin marks on there from when the park was molded. The only extra detail that we're going to add is this loss. So to do this, Let's start a sketch on the front plane. Then go to a normal to view and choose the slot tool. The version that we want to use is a center point straight slot. This is a slot that starts in the middle and goes out equally in both directions. So start from the origin and draw a slot horizontally out like this. We know from measuring it that this is one millimeter high. We also know that the total length of the slot is 6.9 millimeters. If we use Smart Dimension and try to set the length, we've actually got the wrong length there. We've got the length between the two centers of those curved ends. And we want the total length to get around this. We can hold down Shift when I mentioning this will dimension to the outside of the curve. Hold down Shift, select the very outside here on the left and also on the right. And then we can set that dimension as 6.9. Then I'm just going to use that slot shape to make a cut so you can go to Features extruded cut. We can go through all both. This will cut through all of your model in both directions. And that just gives the connector a little bit of flexibility in the middle there so it can fit into the blocks properly. I'm going to rename that feature as middle slot. And then the final thing we need to add is just a two slots, one on each end. These are perpendicular to that first slot, so we need to start on a different plane. If we quickly hover over the planes, we can see we don't want to start on the front plane. The top plane will be suitable. Let's start sketch on the top plane. Again, you can go to a normal to view. It just makes it a little bit easier to draw the slot. I'm going to choose a slot tool and a center point straight slot again. And I'm gonna start the slot at the midpoint of one of these outer edges. If you hover over the edge there, you should be able to pick up the center point of that line. I'm going to draw the slot out like this horizontally to the side. And then the size of it is one millimeter high, so it's the same as the middle one. There's actually a slot on each side. So before we set the length of this, we can mirror this slot over to the other side. To do this, we'll add a center line and you can do this by going up to the line tool, clicking on the drop-down next to it, and choosing center line. Then start the sensor line at the origin and go vertically upwards. It doesn't matter about defining the top of it because it's just a center line. Then we can use that center lines and mirror that slot profile over to the other side. To do this, go to the Sketch tab, choose Mirror entities for the entities to mirror. This is what we actually want to mirror. So we want to select that slot that we drew. Then for the mirror about point, we can choose that vertical center line. We can see that the yellow previews in the correct place so we can press Okay, and now we have the two slot profiles, one on each side. We can now set the exact length of them. We know that the distance between those two slots is 8.5 millimeters. We can use the smart dimension tool. Again, we can hold down Shift when we're dimensioning. This lets you damage into the outside of an arc and we can add the 8.5 millimeters in and that should fully define your sketch. And then just as a double-check this dimension here, the length of the slot from the end should be 3.6 millimeters. And we can see that I is, we don't really need to add that dimension, but it's just there as a double-check that we've got all the sizes right? And then we can go to Features extruded cut. And again, we can choose through all both. And that will cut both of those slots, one in each end. And again, they just give a bit of flexibility to the connector to allow it to actually compress into the holes. Before I save the part, I'm just gonna go to appearances. And I'm gonna change the color of the part to match the real-life part. I'm gonna stay with a medium gloss plastic and I'm going to go for something like a dark gray. In real life, the part is probably more of a black. But actually if you choose the black, you can sometimes lose some of the details there because the black is a very dark color, I tend to go for a dark gray and it just lets you see the edges and the detail of the part a little bit more clearly, if you need to select it. This part is finished. We can now save it. And I'm going to save it as friction pen. And then just put that number on the end, 30465. So we've now made three of the four parts for the first stage and the next one is fairly similar to this one is also a connector, but just with some small differences. 7. Making the Pin with Bore: The fourth and final part of this first stage is also a type of connector, but it's got this hole in the middle or bore in the middle. So I'm going to call this one pin with war. Let's start a new part as usual. And light with a lot of SolidWorks models, there's a few different ways you could model up this connector. It doesn't really matter which way you model it as long as you end up with the correct end result. From looking at the part, I'm gonna make the widest section of the connected first. And the more that you practice with SolidWorks, the easy you'll find it to just look apart on very quickly assess how you're going to build up. I'm going to start a sketch on the right plane, get the circle tool and draw a circle at the origin. This is 4.7 millimeters in diameter. And then let's do a mid-plane extrude. And it should be 22.7 millimeters long. This is our main pin shape, so I'm just gonna call that feature pin. And then there's also a wider section in the middle. I'm going to start another sketch on the right plane. I'm going to get the circle tool again and draw a circle at the origin that's a little bit bigger. This one is 5.9 millimeters diameter. Then we can do another mid-plane extrude, go to extruded boss base, choose mid-plane. And this one is 9.6, so it's a bit smaller than the entire length of the connector. Then let's just call that feature something like middle. Next we've got the wider sections at the end of the connector. I'm gonna start a sketch on this N face. Get the circle tool and draw a circle at the origin. Because there's n face isn't open. We don't need anything in the middle. We don't need any kind of inner diameter. Let's just get the Smart Dimension and set this circle to 5.25 millimeters diameter. So it's the same size as the outer rim of the pin that we made in the last video. Then it's also extruded blind is 0.5 outwards. Let's call this feature outer rim. And then as before, there's one on each end. So we can mirror this over. I'm going to select the outer rim feature. I'm also going to select the plane that goes down the middle. So for me this is the right plane. And then I'm gonna choose mirror and we've now mirrored that REM over to the other side. Now if we look at the part, there's a cavity on each end. This cavity doesn't go all the way through the part, but we're actually going to add the middle section afterwards so we can cut all the way through. Now, it will just make things a little bit easier in terms of modelling. I'm gonna start sketch on the right plane. You could also just start on the end face here. I'm going to go to a normal to view. And if we look at the par is not actually a fully circular cavity in the middle, It's more sort of a rectangular shape with curved edges. From measuring it, we know that it's 0.85 millimeters from the edge. So I'm gonna select this main outer rim edge. And then I'm going to offset 0.85 inwards. If we go to the end view, you can see that a little bit more clearly, then the width of the cavity is 2.2. I'm gonna go back to the end view. I'm gonna get a sensor rectangle. And I'm going to start this at the origin. I'm going to draw a rectangle that's 2 too wide. Then for the height of the rectangle there, it doesn't really matter as long as it covers the entire circle. I'm just going to grab one of these corners and just drag it around and I'm going to fix it. So this outer circle here that fully defines the sketch. So we're just going to cut out that middle section. So I'm gonna go to Features extruded boss base. And then I'm going to do through all both. And I'm going to choose that center section is a rectangle shape with a curved top and bottom. So we're going to cut something like that. It might not quite look right at the moment because we haven't added all of the other features. But as we add those, it should look more correct. I'm going to rename that feature now as bore cut. And then next I'm going to cut a slot, one on each end. So to do this, I'm gonna start a sketch on the front plane. I'm going to go normal two and get the sensor points slot tool start from the midpoint and the end here. And similar to that pin that we made in the last video, we're going to draw a horizontal slot out like this. And then we have two of these slots. So I'm going to add a center line in the middle of vertical center line. And I'm going to use that to mirror that original slot over to the other side. So we've got one on each side. Then let's make these slots one millimeter high so that the same size as that previous connector. Then the distance between them here is 17.8 millimeters. So remember hold down Shift to dimension between the two arcs. Then we can do an extruded cut through all both. And that cuts those slots on both ends. And now you see if we look at the end, it looks a little bit more correct. It looks closer to the real lego part. I'm gonna call out feature slot cut. And then we only have to add that ball in the middle. We can start another sketch on the front plane, going to go normal to get the circle tool and draw a circle at the origin about this size. Then I can use Smart Dimension to set this as 7.4. We can use this to make a mid-plane extrude. And the width of this is 7.8 millimeters. That adds that circular section in the middle. Let's call that something like middle body. We're almost there with the part now the next thing we need to do is cut a hole through the middle. So again, start another sketch on the front plane. Use the circle tool, draw a circle at the origin and set the size there as 4.8. We can then do an extruded cut through all both to cut that bore through the middle. Again, it's that same hole size that we've used on a lot of the parts so far. And this just allows everything to fit together properly. Let's rename that hole as middle ball. Now we've just got that wider Renuka to make on both sides. Let's start a sketch on this face. Get the circle tool again. Draw a circle that's concentric to that center section and the diameter of this is 6.1. Then again, we can make an extruded cut and this is 0.75 deep and it's a blind cut. And let's call that something like middle rim cut. All that remains is to mirror that over to the other side. I'm going to select that middle rim cut feature. I'm going to select the plane that goes down the middle. So for me this is the front plane. And then I'm going to press mirror and that preview looks correct. So let's press Okay. And if we spin it around, we can see we've got that correct drinker on both sides. This part is now finished in terms of modelling as usual, I'm just gonna change the color so it matches the real-life part. If we open the Appearance scenes and Details tab, we can see that there isn't really a default color that matches that sort of lime green color of the lego part. So let's choose something similar, just third, generic green like this. Then what we can do is go into the display manager to do this. Click here on the left on the display manager, and then right-click on that green appearance and choose Edit appearance. We can now set at Green, which is a little bit closer to the real life one. I'm just going to play around in here. And I think that is pretty close there. It doesn't have to be exact. As I mentioned in a previous video, you don't have to change the color like this, just makes it a little bit easier to actually make the leg or assembly when you've got all the parts. Finally, let's save this part and I'm going to call it something like friction pen width bore, and then put that number on the end, 30465. Now we've created those first four parts that we need for that first assembly step, and we'll start putting those together in the next video. 8. Creating the first Subassembly: Now that we've created those first four part, we can use them to make an assembly of the actual Lego helicopter. The first thing that we need to do is make sure we've got all four of those parts open. You can either just drag them into SolidWorks or you can open them in SolidWorks normally. Now once you've parts are open, you can switch between your open windows by pressing control and tab. You see we've got all four of them open. Now before we actually start making the assembly, we need to just have a little thing about which part we're going to start with. You might think that the best one to start with is this large side part of the fuselage, the large right angle beam. That actually if we look ahead in the instructions, we can see that this green connector is right at the center of the model. It's probably best if we line that up with the center of the assembly. This will just help us later on if we need to mirror it any parts over to the other side. Go to this green friction pin with ballpark. Then from within that part, Let's go to File make assembly from power. We're now taken to an empty, blank assembly. And you should see you for open documents here on the left. And these are just parts that are open in SolidWorks. So if you don't see your parts there, you can just click Browse here at the bottom and you can find the parts wherever they're saved on your computer. So firstly, we need to select the part that we want, which is the friction pen with ball. Left-click to select that. And then I'm going to go down a little bit and I'm going to select Graphics preview hit. This just means that when we move the mouse into the graphics area, will be able to see that following the mouse around and see where it will be positioned. Now let's make sure that part is rotated to the correct orientation. You should see this small rotate menu and you can use these buttons to rotate your part by 90 degrees in different directions. If you don't see that menu, to scroll down a little bit and make sure you have a check mark in this box. Show rotate context toolbar. Let's rotate the part around so it matches the orientation in the Lego instructions. We want this hole through the middle, it to be pointing directly upwards instead of pointing forwards. So we want to rotate around the x-axis. So I'm gonna click this X button. And now that hole is facing directly upwards. And then let's place this part anywhere in the graphics area by left clicking. This part is now inserted into the assembly and we can see that it's fixed because there's a small f in brackets next to the part in the parse tree. Also, if we try and drag the part around, we get a small message that says the components fixed and it can't be moved. However, if we go to a top view and we looked at the default planes, we can actually see that the right plane isn't lined up with the middle of the par. So this isn't really what we want. We need to make it. So this part is free to move around and then we can put it in the right place and fix it there. To do this first, go over to the friction pin part with ball on the left and right-click on the part. And from the menu choose float. This will unfixed the parts so we can now move it around. And we can see that the F for fixed as disappeared from next to the part name and it's now being replaced by minus, which means the part isn't fixed. We can now expand the part and we can line up the planes from the part where the planes from the assembly. Let's start off with the front plane from the part. So select the front plane and then hover over the default planes in the assembly. And there should be one that's roughly lined up with that front plane. So in my case it's the top plane. If we hold down control, we can select both of those planes, the front plane from the part and the top plane from the assembly. Then if you release control, we can add a coincident mate and that will align those two planes up. Then let's choose the next one, the top plane in the pot, and then hold down control and select the front plane in the assembly and then release control and add another coincident mate. And then finally, let's do the same with the right plane in the power and the right plane in the assembly. Now we can see that we no longer have that minus symbol next to the partnering. Now it is fully defined. And we can also see it says fully defined down here on the right. Now if we go to top view, we can see we've got the right plane of the assembly at the middle of that part. This will just make things much easier if we need to mirror over any parts from one side of the chopper to the other side. Now that we've fixed that first part in place, let's insert the remaining three parts. You can do this by going to the Assembly tab and choosing insert components. We can see we've got those other parts open there. Again, if you don't have them there, you can click Browse and just find them on your computer. Now before I insert the parts, I'm just going to click on this pin icon here. This just pins this menu open. So it means we don't have to reopen it every time we want to insert a new part. Firstly, I'm going to insert the axial part. I'm going to use those rotation buttons to just rotate it around so the correct orientation. So it lines up with the Lego instructions. And then I'm going to left-click to place it in roughly the correct position. You don't have to rotate it at this stage, it just makes things a little bit easier when we add the mates later on. The next part I'm going to insert is that corner beam. And again, I'm gonna rotate it round to the correct orientation and then place it in roughly the correct place. Then finally I'm going to add the friction pen and again rotate it round so it's in the correct orientation. And then when you're done, you can press OK to close that insert components menu. Now we can see we've got all the parts that we need in the assembly. The only one that is fixed is the green one. The other three parts of Ogata small minus next to them in the street. And that just shows that they're not defined. And we can move them around in space. Now we can start to add some mates to fully define those other parts in the assembly. With Lego is fairly easy to see how parts fit together, so the mates are fairly easy to add. For the first one, let's attach the beam to the sensor connector. All we need to do is select a circular edge of the peg on that connector. Then select a circular face or edge on the corresponding hole that goes into on the beam. Remember if you hold down control, you can tell that these multiple items we know from the instructions that the whole we need is the fifth one along from the front. So it should be this one. When you have your two circular faces or edges selected, release control. And then from the menu that pops up, we can add a concentric mate, which is this one with two circles on it. If you can't see that pop up for any reason, you can also choose the mate tool up here on the Assembly tab, and then you can add a concentric mate there. Now that we've added that first concentric mate, the hole in the beam is lined up with the peg on the connector. But we can still rotate the beam and we can still move it in and out. So we need to add more mates. Firstly, let's zoom in and let's choose that flat face on top of the connector. Hold down control, and also choose a corresponding face on the beam. I'm going to choose this large flat face on the top of the beam. We're gonna release control and then I'm going to add a parallel mate. And then finally, let's just move the beam in to the correct distance from the connector. If we spin the assembly round, we want the outside of the connector to be lined up with the outside of the beam. So let's select those two sets of faces and adequate incident mate. Now we can see here next to the corner being part in the parse tree, we no longer have that minus, so that means that part is now fully defined. We can also expand the mate's folder here at the bottom, and we can see all of them makes that we've added if you need to adjust them or delete them for any reason. Now it's just a case of adding the mates for the remaining parts. Next, let's move on to the actual. At first glance, this one looks a little bit tricky because of the shape. But actually if you remember, these top edges are curved. We've also got the curved edge in the corresponding hole on the beam. We can line those up using a concentric mate. Again, I'm going to select that curved edge on the axle. Also select a curved edge on the beam, then add a concentric mate. Now if we move the actual around, we can see that it can actually still spin around in the hole, and that wouldn't be able to happen in real life. We need to lock the rotation of it. We can do this pretty easily just by selecting one of the flat faces on the axle and then selecting a corresponding flat face on the whole in the beam. Then you could add a parallel mate. In terms of the left, right position, we want the axon to be completely lined up in the sense of the assembly. What we can do is expand the axial part on the left in the parse tree. Then let's find the plane that goes down the middle of the axle. That should be the front plane. Then let's make that coincident with the corresponding plane of the assembly, which is the right plane. And now we can see that the axial is also fully defined and it's lined up in the center of the model. Then finally, we'll just add some mate so that final friction pin connector, I'm gonna move it to roughly the correct place. I'm going to select a circular edge on the pen, hold down control and also select a circular edge on the whole leg goes into, and then we can add that concentric mate. And then on the bottom here I'm going to select this face on the pen, and then this face on the connector. I'm going to make those coincident. Now if we look in the parse tree, we can see we've still got a minus next to that friction pin par. That means it's not fully defined. And that's because we haven't actually locked the rotation. That pain can still spin around within the whole, this doesn't really matter within the model, but if you want to lock it in place just for completeness, then you can do that pretty easily just by adding something like a parallel mate between one of these straight edges on the pin and say a straight edge on the beam. Now we can see that all four of our parts are fully defined. And then down here on the right, it says the whole assembly is fully defined. Now, well done. We've completed the first stage of the Lego chopper. At this point, we can save the assembly by pressing Control S or clicking the Save icon. And I'm going to call it something like stage one, Lego helicopter. Just because it's the first stage of the instructions. And then I'm also just going to add that number that we've added to all of the other parts from the kit, 30465. So we have our assembly all saved there and we've completed the first stage. In the next section, we'll move on to stage two of the instructions. And for that we'll be creating three new parts, but two of them are very similar to parts that we've already created. We should be able to make those pretty quickly. 9. Creating a Longer Axle Using Configurations: This was where we previously left our assembly. We complete the first stage of the Lego instructions. So now we're moving on to stage two. And if we look at that in the instructions, there's actually a smaller sub stage within it that we add to the first stage, we also need to create three new partners. We need a longer axle, we need the right angle beam, and then we need the small bush that fits onto the axial. Let's start off with the simplest one, the axial. If we look at the parts closely, we've actually already created the actual shape that we used in the first stage. We just need to increase the length of it for this version. But what we can do is create a configuration within the axial part. This allows you to have multiple versions of the same part within one single-part file. To get started with S, Let's open the existing actual file, the one that's three long. So you can click on it in the assembly and press Open, or you can just open it directly from where it's saved on your computer. This is the axle that we've already made. It's three bricks long. We now need a version of this that's six bricks long. It doesn't really make sense to make an entirely new part because the only thing that's going to change is the length. Instead, this is a great example of when you can use configurations to make the configurations. First we need to go to the Configuration Manager. That's this tab up here. So click on the configuration Manager tab. We've got one default configuration under that. That's just the standard part. Every part starts with one default configuration. Before we add any new configurations, Let's rename this default one. You can do this by doing a slow double-click on the name where it says default. Let's just call that a three long. We still just have that one single configuration. We've just changed the name of it. The next thing that we need to do is add a second configuration for the longer axle. You can do this by right-clicking where it says Axel where the filename is, and then pressing Add configuration. First we need to give a name to the configuration. So let's call it six long and press Okay. Now we can see we've got two configurations and you can select which one is active just by double-clicking on the name. At this stage, both of our configurations are exactly the same. So changing between them weren't actually changed how the model looks. What we need to do now is go into the sixth configuration and adjust some of the parameters to make it different from the three configuration. So double-click on the sixth configuration to make sure it's active. Then let's go back to the design tree and we can adjust some parameters. The only thing that we need to change is the length of the actual. We can do this by editing that boss extrude feature, the first feature, click on it and press Edit Feature. We can now change the length of this extrude, but just for this configuration, before you actually change anything, let's go down here to the bottom, and let's change from all configurations here to this configuration. That means any changes we make to the length or anything else in the extrude here will only apply to this configuration that we're currently in. We can then adjust the length here. So let's change this to 47.5 millimeters and then make sure you've got this configuration selected and press Okay, now we have that longer axle there. And if we now go back to the configuration manager and we double-click on the three configuration. We should see that the three axial is shorter. And then we can double-click on the six and the six axial is longer. This is a really great way to save time by having different versions of the same part within one single-part file. The final thing that we're going to do is just change the appearance of that longer axle so that it matches the real-life par. To do this, let's make sure we're in the sixth configuration. So double-click on the name and then go down here to where it says display states. Right-click on the default display state. And then let's choose Add display state. So we're just adding a new display state here. We now have to display states, the original default one and the new one we've just added. Let's right-click on that new one and press properties. We can then change the name so it says six loan. And we can also check this box. It says link display states two configurations. It just means whatever display changes we make in this configuration will only apply to this configuration. Then press okay, and now we've got our specific display state just for this configuration. Now we can go and set the appearance in the appearance scenes and Details tab here on the right. Let's expand the appearances. Let's stick with the medium gloss plastic and let's make the axial dark gray. Now the longer axle is the correct dark gray or black color. But if we go back to the three axial, the short racks or we can see that still also the correct gray color. And that's all there is to it really. So it's quite a simple part. You can now save this part. And then in the next video we'll be creating the next part of the right-hand beam. 10. Making the Right Angle Beam: The next part that we need is another right angle beam. It's similar to this one, but it doesn't have the diagonal corner there and it's not quite as complex. But what we can do is actually use that original part as a starting point and just make some changes for this new power. Let's open that original corner being part. You can either click on it in the assembly and press open part or you can just open it directly. Before we make any changes. We're going to re-save this part as a new part. To do this, we need to go to File Save. At this stage, you might get a pop-up like this. We want to choose save as copy and open. This will save the part as a copy, so we'll keep the original part and then it will open the new file so we can edit it there, select, save as copy and open. Now if you don't get this pop-up, don't worry, you can just open the usual save our Xbox. And then we can select save as copy and open from down here on the left is the exact same option. We want to change the name of this from corner beam to something like right-angle beam. And let's change it to four-by-two because it's got four holes along the bottom and two other side before you press okay, just double-check that you've got savers, copy and open selected here so that we don't save over the original part. Then you can press Save. And when we go back into the part, you should see the filename at the top now says right angle beam four-by-two. You may also get a pop up asking if you want to keep the original document open, this is up to you. I'm going to close it in this case, just so don't get confused and make changes to the wrong one by mistake. We can now edit this part and we can make changes to create the new part that we need. The first thing I'm gonna do is drag the robot bar up to the first feature. You can do this by hovering over this blue bar at the bottom of all the features, you get this little hand symbol. And then left clicking and dragging and moving that bar up. Let's drag it all the way up to below that first feature, the beam feature. This moves us back to that first feature in the model. We can now edit that first feature and we're going to edit the sketch that underlies the feature and makes up the feature. To do this, click on the feature in the design tree and then choose Edit Sketch. If we look at the sketch here, we can remove a lot of the detail and we can adjust it so it suits that new part. Let's start deleting the areas that we no longer need. We don't need this slot here on the right-hand side. We also don't need those circles. We don't need this slot here as well. We can change this angle from 135 degrees to 90 degrees, and that'll give us that right angle edge. Then we can use Smart Dimension to re-add some dimensions in. We need to add eight millimeters between these two holes on the right. And we can see that we've lost either the dimension or the relation that fixes the size of this hole. We can select that circle, and then we can select the original circle and we can make those both equal. This is looking almost correct. Now the sketch is fully defined again, is just that bottom edge is too long. It has seven holes and we only need it to have four holes. If you remember back to that early video, we added all these extra holes by using a pattern. We can edit the number of holes in that pattern. To do this, have a look around the pattern and you should see a number seven somewhere that indicates those seven circles that we patterned. If you can't see that number anyway, you can just click on any of the pattern densities, so any of the circles. And then you can right-click up here where it says pattern. You can press Edit Pattern and then we can adjust the pattern there. But a much easier way is just to find that number, the number of instances in the pattern, and then double-click on it, and I'm gonna change it from seven down to four. Now we can see we've only got four circles on the bottom there instead of seven. We've also lost that relation on the right-hand side of this law, I'm going to zoom in. I'm gonna grab the center point of that slot and I'm going to drag it in. So it's concentric without right-hand circle. That should fully define your sketch. Now we have the profile that we need to create this new part. Now that was probably only a little bit faster than drawing out from scratch. But we've actually got all the other features already in the model that we can reuse as well. So it's gonna save as time there. Now let's exit the sketch and we should have something that looks like this. We should have these four holes. And then on the left-hand side here, it should be filled in because that's where the cross hole is going to be. The next thing we can do is move down one step. Let's grab the robot. Borrow again, left-click and drag it down one step, It's beneath that act. So Kurt feature, and we can see that we've added in the axial cut without any extra work. So we don't have to redraw all of that shape and cut it all out correctly. However, if you look here on the left, we can see we've got some kind of warning symbol on that feature. And if you expand that feature, we can see the warning is on the sketch. And if we hover over this sketch, it says unable to offset one or more sketch entities. Let's edit the sketch and see what the problem is. Now if we look at the sketch, we can clearly see the problem is because we deleted that profile section on the right. This part of the sketch here on the right has lost all of its references. And you can see some of the colors there or that kind of greeny brown color, which indicates a missing reference. The good thing is we don't actually need that part of the sketch on the right. We can just drag a box around it and we can delete it. So all we need is this part of the sketch on the left, and then we can exit the sketch. And now we no longer have any error messages there. Now we can go down one more feature. So drug the robot bar down again. So again, we've added in those whole surrounds, but we've still got some kind of error on the feature. Again, let's edit the sketch that underlies the feature and see where the problem is. And as with the previous sketch, we can see because we've deleted some of that extra profile. We've got some parts in the sketch which are referencing things that no longer exist. So we can just delete all of these extra entities here on the right. We no longer need them. If you find that you sketch turns blue and becomes undefined like this. You might just need to use the smart dimension tool to add in some dimensions to fully define the sketch again. Then when you're happy, you can exit the sketch and you can see we've no longer got any errors on that feature. The next feature is the cavity cut. So drag down again and we can see something's gone wrong here. This one isn't quite right. Expand the feature and let's edit the sketch underneath it and see what the problem is with this one. Firstly, let's delete all of these extra entities that we don't need on the right. Then let's zoom in and see what's going on with those remaining entities. I've lost some relations and dimensions here. I'm going to use Smart Dimension to re-add in the distance of this line here on the right. I'm going to add in a distance for these circles as well that are fully defined the sketch. Then if we take a close look at the par, it's actually slightly different to the other beam. Some of the areas around the cavity or a little bit thicker than the other part. I'm going to delete that line here. And then I'm going to offset the edge again, but this time is 1.3 instead of one millimeter. And then you'll just need to drag the bottom with a line down so it hits the circle here. For this horizontal alignment can drag it over to the left-hand side so it's out of the way. Then let's finally add another offset line from this horizontal line. This one is also 1.3 and then just drag the right-hand side of the line over. It, hits that circle. The walls are just a little bit thicker around the inside of that right angle bend just to avoid the two cavities merging into each other, you should end up with something like this. It's a little bit of a messy sketch, but we can exit the sketch now and see how it works. If we look around in 3D, we can see that that feature really hasn't worked properly. So what we need to do now is edit the feature itself and select which areas we want to cut out. Click on the cavity Kurt feature and press Edit Feature. And let's just completely clear all of these areas in the selected contours. So right-click somewhere in that box and press clear selections. Then let's reach use the areas we want to count. So we've got this one here, we've got this one here, and then we've got this one here. And also that small section at the top. The depth of the cut is the same as before, three millimeters. So press Okay, and those new cavities are cut and it should look something like this. We can then drag down again to add the fillet is back in. And again on the feature, we've got a warning. So this time let's edit the feature. And we can see we've got some missing edges there from where we've taken out the previous cavities. So we can remove those missing edges and then we can re-add in the ones that were missing. In total, there should be 12 different edges and it should look like this. And then when you're happy, press Okay. Next let's drag down below the mirror feature, and that all seems to have worked correctly. If we spend the part around, we can see we've mirrored everything onto the other side correctly. Finally, let's drag down below the final fillet feature. And we've got a final error because we're missing some edges from the cross shape that we cut out on the right-hand side. Edit the fillet feature, and let's just right-click and press Clear all missing references. Then you can press Okay, and you should be finished. And there we have our new right angle beam is a lot faster than making the original one because we could change all those features. Let's go into the appearance scenes and Details tab, and let's set the color as a dark gray or black. This part is now finished so you can save the part. And in the next video, we've just got one more simple parts to make, and then we can move on to stage two of the assembly. 11. Creating the Small Bush Part: The final part that we need for stage two is called the bush. It's a little stopper that fits onto an axle. And it's very useful when you're working with those axons. Make it, let's start a new part. And let's start sketch on the front plane using the circle tool. Draw a circle at the origin and set the size of it as 4.8. And then we also have a larger circle, which is the outer diameter of the bush. The size of this is 7.3. Then we need to draw that cross shape in the middle of the inner circle. Get the center rectangle tool and draw to censor rectangles similar to how we drew them for the axles in the previous part. The width of that rectangle is 1.8. Then we can add an equal relation between those two different rectangles between the small edges of them. Then we can also select the small edge and we can make it tangent with that inner circle. Then we can do the same for the second rectangle and that should fully define your sketch. So we've got that cross shape in the middle. Next up we want to extrude everything apart from that section in the middle where the axel fits in. So let's go to Features extruded boss base. As usual, we'll use a mid-plane and the thickness of this power is 3.95 millimeters. Then for the selected contours, we want to choose everything apart from that cross-shaped with the rounded edges, that large outer section, these corners sections, also those small wedges, work your way around and get all of those corners sections. And make sure you also get those tiny little wedge sections that give the curve to the inside of the cross shape. When you've got everything, it should look something like this. Press Okay, to create that feature. Now we just need to add one more feature that is a groove that goes around the outside of the bush. To do this, Let's start a sketch on the front plane. Let's get the circle tool and draw a circle at the origin. The size of the circle is 5.8 millimeters diameter. And then we're going to go to Features extruded cut. We're going to do a mid-plane cut. The thickness of it is 1.3 millimeters. And before you press okay, let's check this box. Flip sides occur. This means we'll cut everything outside of the circle instead of inside it. Then press okay, and we should have something like this. That's the completed pop, finish off the power. We can just save it and let's call it small Bush. And let's put on that number, 30465. Now we've got those three new parts that we need for stage two, and we can create that in the next video. 12. Making Stage 2 - The Fuselage: We've now created those three new parts that we need for the second stage. And I've got those all open in SolidWorks. We've got the long axial, we've got the right angle beam, and we've got the small brush. I've also got that stage one assembly that we made open as well. Now if we look at the instructions, stage two is actually a smaller sub stage that is then added to stage one and some more parts are added. So we could just make the entire chopper assembly just as one single assembly. But actually we're going to follow the instructions and we're going to make each of these subassemblies in the instructions as a sub assembly in solid works. This will hopefully just make it a bit easier to understand what's going on and to actually follow the Lego instructions a bit more clearly. So the first thing we need to do is make that small sub assembly with the right angle beam and the longer axle. Let's go to the right angle being part remember you can switch between open documents by pressing control and tap from within that part. Let's go to File make assembly from part. I want to choose the right angle beam four-by-two. I'm going to turn on the graphics preview. And then I'm just going to press Okay to insert that part fixed to the origin of the assembly. Then if we just spend the assembly round, we can see that the part seems to be lined up correctly, so the default planes are going down the middle of that part. We can now insert that larger axial, the sixth long axial to this assembly. You can do that by going to assembly, choose an insert components, and then selecting the actual power. And then I'm just going to left-click and place it in roughly the right position about that. Now if you find when you act or parties inserted that it's the smaller gray one. Or you need to do is left-click on the part in the graphics area. And from this drop-down, let's just choose the six long axon. That drop-down allows you to select which of the configurations you want to use for that part. Now it's just the case of meeting these two parts together. So let's zoom in, select a circular face from the axial, and then also select a circular face from the axial hole in the right angle beam. And let's make those concentric. We also don't want the axle to spin around because that wouldn't happen in real life because it's stuck in a cross shape. Instead of adding those parallel mates like we did with the previous stage, what you can do is just expand the mates or the bottom of the poetry. That's fine. The latest might be only one that we've added that concentric mate. Just right-click on it and then press lock rotation. This just means that that part won't spin around within the hole. Now we've got the actual in the hole, the rotation is locked and we just need to set the left-right position. Let's move it to roughly the correct place. And then let's expand the axial part. Let's find the plane that's at the middle of the axle. So it's the front plane. And then hold down Control and then select the corresponding plane from the assembly. So for me it's also the front plane. And then we can add a coincident mate. Those two planes are lined up. There. We have our small sub-assembly for stage two. So it's a very simple assembly. You can now save this and let's just call it something like stage two, Lego helicopter 30465. Now in SolidWorks, I've got both of those assemblies open. I've got stage one that we previously created, and I've got stage two that we made just now. But actually stage two in the instructions is a combination of this new smallest stage to assembly and the original stage one. We need to make them both into a new assembly. What I'm gonna do is press Control and Tab to go to stage one. And then we can go to file make assembly from assembly. Again, this takes us to a new blank assembly. We can choose stage one here on the left. And then let's press the green tick and that should insert stage one fixed to the origin of this new assembly. It should be inserted something like this. And then if we double-check looking at those default planes, it looks like they are correctly at the center of the model. We can now insert that second sub-assembly. Go to the Assembly tab, go to Insert Components, and let's choose stage two. So I'm going to move that roughly the correct position. You might need to rotate it around using those rotation buttons. And then I'm just going to left-click to position it in about the right place. Looking at the instructions, it looks like it should be roughly about there. We can then add some mates. They're actually properly lock it in place. We can see that they small gray axle needs to go through this third hole on the right angle beam here. Let's zoom in a little bit. Let's choose that circular face on the triaxial. Also choose the circular face inside that hole on the beam. And let's add a concentric mate that moves that sub-assembly, something like this, but we can still rotate it around. You wouldn't be able to do this in real life because the axons would crash against the beam. So first let's select the two flat edges of each of the beams and make those parallel. Then we just need to set the left right position again. We could add a coincident mate between those two faces with BIM that are next to each other. But actually there's probably a small gap in there just to allow the parts to move around. What we'll do instead is we'll go down in the parse tree, will expand the stage to assembly. We will find the plane that goes down the middle of it. So for me this is the front plane. And then we align that plane up with the middle of the new assembly. Line it up with the right plane of the main assembly and we'll make those coincident. Now that stage to subassembly is exactly in the middle of the assembly. And if we zoom in, we can see that there is actually indeed a small gap in-between those two parts. Now the final thing that we need to do for this stage is add that small bushing in place. Let's go to the Assembly tab, go to Insert Components, and then select that bush part. If you don't see it there, you might just need to click browse and find the bush part wherever it saved on your computer. I'm going to rotate it around so it's in the correct orientation. And then just zoom in and I'm going to select a circular edge from the axial and also a circular edge from the bush. And I'm going to add a concentric mate. I'm going to lock the rotation. If I go down to the bottom here and expand the mates, we can see that this concentric mates at the end is the latest one. If you've just got two circles which aren't filled in, in the middle. It means the rotation isn't locked. I'm going to right-click on that May and I'm gonna choose lock rotation. Now if you look at the symbol, you can see the inner circle is filled in. So that indicates that the rotation is locked. Now the bush can't rotate and it can only go along the axon. So the final thing we need to do is just move it into the correct position. Let us choose this outside face of the beam and then this face of the bush. And then let's add a coincident mate. And it should look something like this. And all of our parts should now be in the correct position and everything should be fully defined. We can now save our assembly and let's just call it something like main assembly, like our helicopter 30465. Well done for making that second stage already is looking a lot more advanced than just a few videos ago. In the next section, we're going to move on to stage three. And we need to create two new parts, and then we need to add those to the new assembly. 13. Creating the Long Pin Part: We're now onto stage three. And for this we need to new parts. We need a longer friction pen and we also need across block, which allows us to join a pin and an axle at 90 degrees. Let's start off with a friction pen. And looking at this longer version, it's pretty similar to that first friction pin that we made. So we can use that as a starting point and then we can just make some adjustments to the model. Let's open that original friction pin file. Here is I'm just going to drag it into SolidWorks. And then we're going to save this as a copy and then modify the file. So once the file is opened, the first thing we're going to do is save it as a copy. You can do this by going to File Save As. And then from the menu, Let's choose save as copy and open, which is this bottom one. Let's give it a new name, something like long friction pen, and then press Save. And if you get a message asking if you want to keep the original file open, It's up to you personally, I've closed it just to avoid any confusion with that file. Now we can modify this friction peer modal instead of making the new one completely from scratch, the first thing that I'm gonna do is drag the Roebuck bar up to below the first feature. That first feature is the ring that's in the middle of the pen. And this is actually the same on both the short paint and the long pen. We can just leave this as it is and we can drag down below the next feature, which is the outer body. Now this is where things start to differ a little bit. On the original pin we extruded in two directions equally. But on this longer pain, we want to extrude in one direction and then the other direction needs to be twice as long. All of the other sizes stay the same though the inside and outside diameter. To adjust the width first, we've got to edit this feature. Click on the outer body feature and then press Edit Feature. And let's change the end condition here from mid-plane to blind. Now we're just extruding in one single direction. For the first direction, we're going to extrude 7.5 millimeters. Then we want to extrude twice that distance in the other direction. You can do this by clicking here where it says direction too. For this extrude, we're going to continue with the blinding condition, but we're going to extrude 15 millimeters. So it's doubled the length of the opposite side. So we're extruding one side by 7.5 and then the other side by 15 at one. That looks good. You can press Okay. Now that we've got the basic shape, we can drag down below the next feature, which is the outer rim. That is all the same. We're just extruding that small amount by 0.5 millimeters from the end of the pin. But if we drag down below the next feature, the mirror, we can see that this rim on this side is in the wrong place. We can just completely delete that mirror feature and let's just draw another ring manually. So spin the pen around, start sketch on this end face. Let's choose that inner edge and press convert entities. And then let's choose the outer edge on the other side and press convert entities again, you should have two concentric circles. One of them is the size of the inner diameter and one of them is the size of the outer rim on the other end. We can then extrude that 0.5 millimeters outwards. We should have the overall correct shape there. Now, we can rename this feature as outer rim two, and then we can drag back down below the next feature. This next one is the middle slot. And if we look at the model, this is actually in the wrong position now. It's struggling that wider part in the middle when it should be further over to the right. What we need to do is edit the sketch underneath that middle slot feature. Click on the feature and press Edit Sketch. And I'm going to go to a normal two view. So we can see quite clearly where we're cutting. The size of this law is the same. It's still 6.9 by one millimeter. We just need to move the position. To do this, we need to delete the coincident relation that anchors in place on the origin. Click on the point at the center of this law and then delete the coincident relation. Depending on your view settings, you might be able to just click on the coincident icon and press Delete. If you can't see it there. Then actually click on the center point of that slot. And then you should be able to see the coincident relation here on the left, and you can then delete it. Now that that coincident relation is gone, we can move that slot around and you can see it's turned blue. Let move it to roughly the correct position. So my light here. Then let's set the up-down distance. So to do this, let's select that point in the middle of the slot. And then let's also select the origin and let's make those horizontal. And then for the exact left, right spacing, I've measured it from the end of the pen here. Let's get the smart dimension tool. And let's add a dimension from the end of the pin to the outside curved edge of the slot. Remember you can hold down shift to dimension to the arc that I mentioned. There should be 4.3 millimeters. Then just press Okay. And now we can see that slot is going through in the correct place. Now we can drag back down below the final feature to start in those final n slots. And I'm just going to rename this feature to say n slots. Now if we spin the model around and we looked at those slots, one of the ends looks correct, but the other one the slots in the wrong position. So again, we need to edit the sketch underneath this feature. Click on the feature and then press Edit Sketch. If we now go to normal two view, you can see the one on the right is correct, but the one on the left needs to be moved outwards to the left. So that's also on the outer edge of the pen. To move this lock first, we will have to move the center line that is mirrored about. So click on the center line, click on the point that's fixed to the origin and then delete the relations there. That center line is now free to move around. Next up, we know the distance between this law should be 15.85 from measuring it, I'm going to double-click on this 8.5 and I'm gonna change that to 15.85. And that will move the slots apart. We're still not quite in the correct position though, and we're still not fully defined. So what you're going to have to do is grab the center point of this left-hand slot and then just drag it out. So it's at the midpoint of the left-hand edge of the pen. That should fully define your sketch. This one on the right is fixed at the midpoint of the right-hand edge. And the one on the left is fixed at the midpoint of the left-hand edge. And the distance between them is 15.85. So in this case, because we've got those other relations and dimensions, it means that it doesn't really matter where the position of the center line. It can only actually be in that one position in the middle. Then when you're happy press Okay, and that will create those cars. Then the final thing we need to do is just change the color. Let's go to the Appearance scenes and Details tab on the right. And let's choose a standard blue. And now this part is finished so you can save it. In the next video, we'll be making a completely knee pop the cross block that allows you to join an axial and a pen. 14. Making the Cross Block Connector: The next part that we're going to make is called across block. And it basically allows you to join a pin and an axial at 90 degrees. Now I feel like I say this quite often, but this part really could be made in quite a few different ways. Just for now, I've hidden the design tree, have a look at this part in 3D, and maybe pause the video and have a little think about how you would make this, what steps you would take. Let's actually start modeling and see if we add the same ideas. I'm going to start a new part and start a sketch on the front plane. And I'm gonna start with the part where the pin goes through. I'm gonna get the circle tool. I'm going to draw two concentric circles at the origin. These are for the outer size, which is 7.4 millimeters. And then the inner ball, which is that usual 4.8 that we've used in quite a few parts so far. Then I'm going to do a mid-plane extrude. This part is actually the same width and height. The Extrude is 7.4 as well. This is the area where the pin will fit in. So I'm going to rename this as pin side. Next up looking at the part, I'm actually going to make those little sort of ears that come off the top. To do this, I'm gonna start a sketch on a plane that goes through the middle. So for me it's the top plane. Starts to catch on there and I'm going to go normal too. Then I'm going to get the line tool and I'm gonna draw something like this. I'm going to start at the midpoint here and go down to the other midpoint and then go out to the right-hand side. And then I'm going to start a new line across the top. That's the same as the bottom one. Now we're going to join this open-end using an arc. You can go to the Arc tool and we're going to choose a tangent arc. Start from one of the open ends of the line and go round and finish at the other line. So it's tangent here at the top and also at the bottom. We can then use Smart Dimension to set the size. Let's start here on the very left and go out to the outside of the arc. Again, you'll need to hold down Shift to dimension to the outside of the OK. And let's set that length as 15.4 millimeters. This profile is going to make up that little ear on the top of the part. We want to extrude this area upwards, but we don't want to extrude in the middle of the part. We want to extrude on the very edge of that circular section we've already made. When we make the extrude feature, we can actually offset where it starts from. To do this, go to features and just choose the standard extruded boss base. Firstly, we want to extrude in a blind direction one millimeter, but before you press Okay, Let's offset the start point. You can do this by clicking on this from drop-down here. And let's change it to offset. We can then set the offset on my own. We know that the total diameter of that circular section is 7.4. We want to offset half of that, which is 3.7. So let's write in 3.7. Just before we press OK, we can see we're extruding in the wrong direction. We're extruding upwards. When we shall be extruding downwards, we can correct this just by flipping the direction, by pressing the reverse direction box here on the left. And when your preview looks good, press Okay to make that first year. And I'm gonna call that feature something like side ear. We can then mirror this over to the other side. So select that feature, then also select the appropriate plane. For me, it was the top plane. And then press mirror. The preview looks good. So let's press Okay to mirror that air down onto the bottom. Next up I'm going to draw that rib in the middle that joins the two years together. I'm going to start sketch on the appropriate plane. That's the one down the middle, the front plane here. And then I'm going to go to a normal two view. I'm going to select these three edges and convert them all. And then I'm just gonna draw a line across the middle there to close the profile. We can then extrude that and do a mid-plane extrude. This is Warren, 0.4 millimeters wide. Hopefully you can see we're starting to build up the shape now and I'm going to rename that feature as middle rib. Next up I'm going to add that circular part where the axle goes through. So I'm gonna start sketch on the top plane. I'm going to get the circle tool and go normal too. And I'm going to draw a circle that's concentric with that circular edge on the end. I'm gonna start at the midpoint of that circular edge. I'm going to go out and set the size as 5.7. I can then do a mid-plane extrude, and I'm going to set that as 7.4. So it goes exactly up to the edges that we've already made. And I'm going to call that feature something like axial body. So we're almost there now the next thing we're gonna do is count the cross shape for the axial. Start sketch on the top plane. And we're going to draw and cut out that usual shape that we've done quite a few times. Now, get the circle tool. Let's draw a circle that's 4.8 millimeters diameter. Then get the center rectangle. We'll draw our two center rectangles, will make the rectangles the same width, which is 1.8. And then we'll add those tangent relations to join the rectangles with the circle. When you've done both of those, we can do an extruded cut. We can go through all both, and we can choose those usual five sections to cut out that cross-shaped actual area. Then I'm going to rename that feature as axial cut. The next thing we need to do is cut a slot through the middle of the axial section. You start sketch on the front plane, get the slot tool. I'm going to get a center point slot, and I'm gonna draw a slot somewhere in roughly this position. We can set the position mostly using relations. So firstly, let's select the origin. Let's also select the center point of the slot, and let's make those horizontal. Then let's get the center point of this law. Again. We're line that up with this edge above here. You might need to add a coincident. Now you might be able to use a vertical depending exactly what you select. Then let's select the outer arc of this law, and let's make that tangent with this lower edge here. And then finally, let's set the width of the slot has one millimeter and that should fully define your sketch. If it doesn't, you might just need to add in a few more relations or dimensions to do that. We can then use this large shape to do an extruded cut through all both. And we can call that feature acts or slot. Then we've just got one final set of features to add that wrinkles around where the pin goes in. So let's start a sketch on this face. Get the circle tool, and draw a circle at the center point of that whole. Let's set the size of that as 6.2 millimeters. And then just do an extruded cut blind 0.8 to cut that little rim section. I'm going to call that one pin rim. And then we can just mirror that over to the other side to finish the modelling. So select the pin rim, also select the appropriate plane. For me, this was the front plane. And then if the preview looks good, Let's press Okay to create that mirror and we now finish modelling. So actually in the end the part wasn't too bad. We just went through it logically and built up out of simpler features. We can now open the Appearance scenes and Details tab, and we can add the appropriate color, which is dark gray or black. We're now totally finished, so we can save this part. Let's call it cross block 30465. In the next video, we'll take these two new parts and we'll use them to complete stage three. 15. Building Stage 3 - the Upper Fuselage: Now that we've created those two new parts, we can move on to stage three before we actually start making it. Make sure you've got all the documents we need open. So we've got the original main assembly, we've got the axial part, we've got the small bush part, and then we've got the two new parts that we just made, the long friction pen and the cross block. Looking at stage three, there's actually a smaller sub stage that we're going to make first, let's start off with our crosswalk piece. I'm gonna go to the crosswalk piece and then I'm going to go to File make assembly from part. We're now in a new blank assembly. I'm going to choose that cross block part and then press Okay to insert that part fixed to the origin of the assembly. Next, I'm going to insert those two other parts that we need. So I'm going to go to Assembly, insert components. And before I insert them, I'm just going to pin that menu open. Firstly, I'm going to insert the axial, something like this, and I'm going to switch that around so it's in the correct orientation and make sure you've got the actual lists six loan. Then I'm also going to insert that long friction pen. You might also need to rotate that around. You can then close the insert components menu and we'll start to add some maze. Let's start off with the axle. I'm going to select a circular edge of the axle and then a corresponding circular edge on the cross block. Then I'm going to make those concentric. I'm going to lock the rotation of the axle. So you can do this by expanding the mates. We can see that the concentric mate isn't locked because the circle isn't filled in in the middle. So we can right-click on the mate and we can press the lock rotation. And now you can see the circle is filled in in the middle. And then I'm just going to send to the axis, I'm going to move it to about the right position. I'm going to expand the axial part in the street and find the plane that goes down the middle. And then I'm going to make that coincident with the plane that goes down the middle of the assembly. The axle is all fixed in place. Now if we look at the instructions, the orientation should be something like this. Next step we need to put the pin into the hole. We need the large section of the pin facing upwards. So as we look at it at the moment, the pin is 180 degrees outlets in the wrong direction. If you do have it in the wrong orientation like this, you can either just rotate the part by holding down the right mouse button and dragging the part around, something like this. What you can do instead say you in this position is you can just add the concentric mate the wrong way round like this by selecting the two circular edges and adding the mate. Now we've got that concentric mate boats in the wrong direction. If you find that concentric mate and then right-click on it, you can then press Flip Mate alignment that will spin them around to the opposite direction. So it should be something like that. Then let's add another mate. So let's rotate the whole assembly around. Let's add a coincident mate between the bottom of that long friction pen and the bottom of the cross block. And then if you want, you can just start a final mate to stop that long friction pins spinning around. So you can maybe select a straight edge and then another straight or Jim across block and make those parallel. We can then save this stage. So let's press Control S. And this is stage three of the Lego helicopter. We can now add stage three to the main assembly. I'm going to press control tab to switch between my open document. And I'm going to go to that main assembly that we've already been working on. Now let's insert that new stage three sub assembly that we just made. So go to these empty tab, choose Insert Components and find stage three, and then left-click to place it somewhere in the graphics area. And if you want, you can rotate it around to the correct orientation. Just looking at the instructions. It should be something like that. It doesn't matter too much if you don't get it right before you insert the subassembly, because you can just rotate it around by holding down the right mouse button and dragging the subassembly around. Now let's make this in the correct position. So let's choose a circular edge here. Let's choose the corresponding edge in the beam and add a concentric mate. Let's just drag it to about the correct position, which is about here. Then let's make the top of this cross block parallel with the top of the beam. Then we've just got to set the left, right distance. So we want a exactly in the middle of the assembly. So perhaps we could make one of these edges coincident with one of the edges of that front beam. But what we'll do is we'll use the planes just to ensure that it's exactly at the middle of the assembly. Expand that stage three subassembly in the parse tree, then find the plane that goes down the middle. So for me this is the top plane. And then just line that up with the corresponding plane in the assembly, which for me is the right plane. And so I'm gonna make those coincident. So we're really starting to see that shape of the chopper fuselage coming out. Now, the last thing that we got to do in this stage is add one more of those Bush parts. Now you can just go to Insert Components and then find that part and insert it. If you spin the model around, you can see we've actually already got one of those parts. We can just copy it from the assembly to add a new one. You can do this just by holding down the control key and then left clicking and dragging from an existing part. Then release the left-click and you should insert another copy of that part. We can then make this in position. So I'm going to select a circular face on the bush, also a circular face on the axle and make those concentric. I'm going to lock the rotation. I'm just going to expand the Mates here on the left. I'm going to right-click on the latest concentric one and press lock rotation. Then I'm just going to select this outer face of the beam and the interface of the bush and make those coincident. So stage three is now complete. In the next video, we're moving on to stage four. We need to make two new parts. They're both quite simple beams, so they should be pretty quick to make. 16. Building the 7-Long Beam: We're now moving on to stage four of the instructions. For this one, we need to make two new parts and they're both pretty simple beams. What we're going to do is open one of those early parts, the corner beam, and then we're going to re-save that as a copy and modify it. Let's open this original corner being par. When you've got it open, Let's save it as a copy by going to File Save As. And then choose save as copy and open that I'm going to change the name and it's a beam and it's seven long, so I'm gonna call it BIM seven long. Just as a double-check, make sure you've got savers copy and open, and then press Save. You can then close the original file if you want to go into modify this part in a similar way to how we did with some of the other parts. I'm going to drag up the robot B2 below the first feature. You don't have to do this. Sometimes it just makes it a bit clearer to see what exactly you're working on. Then I'm going to click on that first feature and I'm going to edit the sketch underneath. For this one is just a single beam. It's got seven holes, so we don't need any of this stuff on the right, so you can drag a box around that and delete that. All we need is this along the bottom, and that's really all there is to at this stage, you can exit that sketch and you'll probably see something like this. Now, actually, if we look at the part, we do want to extrude the hole on the left. So what we'll need to do is edit the actual feature this time instead of the sketch. So edit that being feature. And then in the selected contours, just clicking this box so it's active. And then just click on the inside of that circle on the left to de-select it. We want to extrude something like this. So it's a beam with seven holes in it. Then we can drag down below the next feature. This is the actual curve, or in this part we don't actually have an axial cut. We can just completely delete this feature. So I click on it and press Delete. And you can also delete the sketch that's underneath it. The next we can add the whole surround. So let's drag down again. We can see we're missing one of the whole surrounds on the left. And we've also got some kind of warning on the sketch. Let's click on that feature and let's edit the sketch underneath that. Now if we go to a normal two view, you can see we can delete all of this stuff on the right that we no longer need. When you remove those, your sketch might become undefined. So if your entities turn blue like this, just use the smart dimension to add in another dimension. Then I'm just going to get the circle tool and I'm going to add another circle on the left here where it's missing. Draw a circle there. I set the rough size and then select that circle and one of the other circles that's already fully defined and make those equal. We should have something like this. All of the holes, I've got those wider circles. You can then exit the sketch. And we should have all seven of those holes around cars. Then we can drag back down below the next feature, the cavity gut. Again, we're missing a cavity on the left and we've got some kind of warning on the feature. Let's click on a feature and edit the sketch underneath. If I go to a normal to view, again, we can delete all the stuff on the right that we don't need. If you lose any dimensions, just re-add those in. Then all we need to do is just add one more large circle here on the left. You can use the circle tool to do that and you can make it the same size as the other ones by using that make equal relation, your sketch should look something like this. So let's exit the sketch. If you find that the feature isn't created properly like mine here. What you can now do is edit the cavity coat feature itself. So click on the feature and press Edit Feature. And then in the selected contours box, just clear all of the existing selections. And then choose those gaps between all of the holes. We're going to be cutting the same depth, which is three millimeters. When you've got all of them selected, just press Okay to make that cut. Then let's drag down again below the filler. We can see we're missing fillets here on the left. We've also got a warning on the fillet feature. That's because we've removed some of the edges that were previously filleted. Click on that, fill that feature and press Edit feature. For me, a warning popped up that said we're missing some edges. These edges have been automatically removed from me. If you have edges in the box here on the left, I've got warnings, then you can just delete those manually by selecting them and pressing Delete. And then it's just a case of adding those for extra edges on the left here. We should have all of those internal edges and then press Okay, and that feature is made. Then finally we can drag down below the last feature, the mirror, and we can see that everything is being mirrored correctly onto the other side. So this part is finished in terms of modelling. Now let's just change the color as usual. So open the Appearance scenes and Details tab. Let's choose a green color, which is pretty close. Then let's go to the Display Manager and edit that appearance. And let's change the color to be a bit closer to the real life one. And then this part is complete so you can save it. In the next video, we'll be making a very similar part to this. It's basically the same part of it. It's only five long instead of seven long. So that should be a very quick one. 17. Making the 5-Long Beam: In the previous video, we created this seven long straight beam. And in this one we're just going to modify this. So it's only five long. As with the previous video first, we're going to save this as a copy. Open the seven long beam, and then go to File Save As. And we want to choose save as copy and open. Let's change the name from beam seven long to beam five long and press Save. Now we just have to make this part a little bit shorter. So as usual, I'm gonna go back to the design tree. I'm going to drag up to that first feature and I'm going to edit the underlying sketch on that first beam feature. I'm going to click on the number of instances here where it says seven. And I'm gonna change that from seven down to five and press Okay. If you can't see that seven anyway, you can just click on one of the circles. And then here on the left you can right-click on the pattern relation and you can press Edit Pattern. And then we can change it from seven pounds a five there and press Okay. Now we only have five holes and we've also lost the relation on this right-hand side of this law. I'm going to grab that center point on the right and I'm gonna drag it in. It's concentric with that right-hand circle. Then let's exit the sketch and you can see we now have a beam that's five long necks. We can drag down below the next feature, the whole surround. Let's edit the sketch that makes it this feature. And let's just delete those two extra holes on the right. If you find that your sketch turns blue and becomes undefined, you might just need to add some more dimensions in there. Let's exit the sketch and we've now got that whole surround on those five holes. We can then drag down below the next feature, the cavity cut. Again. Let's edit the sketch which is underneath the feature. Then let's delete those extra two circles on the right and exit the sketch. If you find that your cavity curtain now isn't made correctly like this, you can edit the cavity cut feature. You can then clear all of the items under the selected contours, and then just re-select those cavities in the middle. Then drag down again for the fillet. Again, let's edit the feature and let's remove any missing edges there. Then press okay, and that's all looking good. We can drag down below the final feature in the mirror, and we can see that we correctly mirrored the items onto both sides. This was a very quick part of the final thing we have to do is just change the color to white. So open the parents scenes and Details tab and choose a white color. Then you can save the part. And in the next video, we'll be adding these two new parts to stage four. 18. Stage 4: Creating the Tail Boom: Now that we've made those two new beams, we can complete stage four. Got that main assembly open. I've also got those two new beams opened. First, I'm going to insert those new part into the main assembly, goto Assembly, insert components. I'm going to pin this menu open. First. I'm going to insert the five long one and I'm gonna spin it around so it's in roughly the correct orientation like this. Then I'm going to insert the seven and they're gonna spin it around as well. We can then fix these in place using some mates. The first one is the small white one. So let's zoom in a little bit. Let's select this circular face. And then let's select the corresponding long face on the friction pen and let's make those concentric. Next up, we should also be able to make the long blue pen concentric with one of the holes further back on the beam. So let's choose those two circular faces and make those concentric. You can see that lines at the beam. So it's in exactly the right orientation. Then let's just choose the bottom of that short beam and then choose the top of that green connector. Let's make those coincidence. So we've now added that being part in place. Next up, if you look at the instructions, we actually need to add another of those small black friction pins. We'd like you instructions. It can be quite easy sometimes the mess these little steps. But I think that's sometimes kind of part of the fun trying to figure out what you missed and why something doesn't fit together or why you've got some extra parts leftover. We need to add another friction pen to do this, you can't find the file on your computer and insert it directly. We can just copy one from the assembly already. To copy it from the assembly, Let's hold down the Control key and then left-click and drag from one of the existing pins. And then just release the left mouse button to place that new pi. Then going to make that pin into this hole at the back using concentric mates. I'm going to set the position like so by adding a coincident mate on the bottom here. Then I'm just going to lock the rotation. I'm going to go down to the bottom of the parts tree. I'm going to expand the mates. I'm going to find that latest concentric mate, which is this one. And I'm going to right-click on it and I'm going to press lock rotation. And then we just have to position this long green beam at the back. First, let's add a concentric mate between that first hole and the blue pen. You can see now we can actually move up and down and we can rotate around as well. But if we add another concentric mate here between this black pen and the second hole, we can no longer rotate. We can just move up and down. Then to fix the up and down movement, Let's just choose this top face of the beam and then the corresponding face on the green beam and make those coincident. And then stage four is now complete. So we've started to build up that tail section on the back of the chopper. At this point, you can save your assembly. And in the next video we'll be going onto a stage five and making one new part. 19. Making the One-Sided Pin with Bore: Welcome to stage five. This is a pretty quick stage. We've only got to make one new part. We've actually already made most of it for another part. It's very similar to this friction pen with ballpark that we've already made. So let's open that part. You can either open it by clicking on the file directly or you can go to the Assembly, click on the part in the graphics area and press open part. Now we basically want to make this exact same pen, but we only want one of these arms coming off it. We don't want both of them. So we could just keep this one and then cut one side off. But it's probably a little bit less messy to adjust the original features. First, let's save this part as a copy from within this part, Let's go to File Save As, Let's choose save as copy and open. So make sure you have save as copy and open selected down here. And let's rename the part. Let's call it something like one-sided friction pen width, ball, and press Save. I'm going to close the original part and then make some small changes to this part. If you remember when we made this pin first, we made that long center section. And we did this using mid-plane extrude. We need to just modify the original center section instead of going out in both directions, it only goes in one direction. To start off with this, Let's edit that first feature, the pin feature. Firstly, we don't need to go in both directions. So instead of a mid-plane, we can change it to blind. Also, we only need to extrude half of the original distance. Originally it was 22.7. So we just need to have that. If you're not too hot on maths. And easy way to divide this by two is to just click in the box. And then after the number, just slash two and then press Enter. This will divide that number by two. That's now being divided by two is 11.35, without us having to do any of the maths. Then let's press Okay to accept that feature, Let's do the same for the next feature. I'm going to edit this middle feature. I'm going to change it from a mid-plane to blind extrude. This means we're only extruding in warm single direction. And then I'm also going to half the amount that we're extruding. I'm going to click after the number in the box and I'm gonna put slash two and press Enter. And that will divide that number by two. And then I'm going to press Okay to accept that feature. Then let's drag down again. We've got the same outer rim so we can just leave that. Then if we drag down again, the mirror features got an error on it. But we don't actually need this mirror feature because we've only got one side. We can completely delete that. Next, Let's drag down again to add the walker. And with this, you might find that you get an error. If we click on that feature, we can see the error says cannot locate the end of the feature. Let's edit that feature and see exactly what the problem is. Now the problem is we're trying to cut through all both. But the sketch is actually right on the end of the part already. So there's nothing for it to cut on the left-hand side. So SolidWorks is getting a bit mixed up here. To fix this, Let's just uncheck this direction to box. Now we're just cutting through all in one single direction. You might need to flip the direction by clicking the reverse direction box here. Now we can see the previews working correctly. We're going through all the model in the correct direction. So you can press Okay to make that cut. Let's drag down again below the next feature and the slot cut has been created properly. If we actually look at the sketch underneath, we've still got that slot on the left-hand side. But because there's nothing there, It doesn't really matter that there's nothing to cut there. So we can just leave that as it is. Next, we can drag down again. So there we've got the middle body. We can go down again. And then we've got the whole or the boar through the middle. Then for the next one we've got the outer rim curr, and then for the final one, the mirror with mirror that Renuka onto the other side. So that's that part complete and it's already the correct color. So we can just save that. In the next video, we'll be putting this part into stage five of the assembly. 20. Stage 5: Adding the Tail Rotor Transmission Housing: We're now onto stage five, and this is a pretty fast one. We only need to add two new parts. The first one of those is this existing friction Pim with Bohr. Let's hold down Control. Left-click and drag from that part in the graphics area, and then release the left mouse button to add a new copy of that part. Then the second part is that pin with just one side that we just made. You can insert this by going to Insert Components and then finding the file on your computer. So that should be called one-sided friction Pim with board. And before I insert it, I'm just going to spin it around so it's in the correct orientation. I'm going to add mates to this left-hand part first, just to make sure that we get the holes lined up correctly between the two new green parts. I'm going to select the hole on the beam and the circular face of the peg and make those concentric. Then I'm going to drag the part out. And actually we want this hole in the middle to go along, so we might need to rotate it around a little bit. It should be in this sort of orientation. Now to make sure this is lined up correctly, Let's click on the part. We can now see you in the street and we can expand the power. And then let's select one of the planes down the middle. So for me this is the top line. We can then make that plane parallel with one of the top faces of one of the beams. This just means that that hole is lined up correctly. We know that the par isn't twisted. The next thing we want to do is make sure that hole is exactly in the middle of the model. Now with some of the parts we lined up the outer face with the outer face of the beam. But with this part is really important that the whole goes down the middle of the model. So what we're gonna do is expand the part again. We're going to choose the plane that goes down the middle of the part. And then we're going to make that coincident with the middle of the assembly. And then that front part should be fully defined. We can now add some mates to that final part on the right-hand side. First, I'm just going to line up the peg on the bottom with a hole in the back of the beam. I'm going to make those concentric. And then I'm gonna select the board that goes through the middle of this front pin. And also select the board that goes through the middle of the back pen and make those concentric. This is where the actual we'll go through that actually runs the tail rotor. So it's important that these aligned up. And we can see that we only actually needed to make a fully defined that part of the back. We can then save the assembly and stage five is done. In the next video, we'll start on stage six, which includes modelling up and adding some gears. 21. Creating the 9-Long Axle Part: We're now onto stage six. And for this we need to make three new parts. So we need a longer axon or larger bush. And also we need to make the gear, which is fairly complex. But we'll start off with the simplest part, which is the axle. To make this, let's open the existing actual power. You can do this from within the assembly by clicking on the axle and pressing open part. Or you can just open the part directly by double-clicking wherever it saved on your computer. This will be a very quick part to make. All we need to do is add another configuration with a different length. So you might remember if we go to the configurations manager, we've got those two existing configurations. We've got the three long and we've got the sixth long. We now need to add a nine long. I'm gonna make the three axial active by double-clicking on it. Just because it's the same color as the axon. When you add a new configuration, it's based on the one that you currently in. Make sure you have the three active. And then right-click on the file name at the top here, and then choose add configuration. And then let's call this 19 long and press Okay, Make sure you in the nine long configuration. So it should be active here and then go back to the design train. Now it's just a case of editing the length of that first feature. Let's click on the existing boss extrude feature and choose Edit Feature. Now we just need to change the length before you do just double-check that down here under configurations, it says this configuration, they should be automatically selected. This just means that any changes we make now will only apply to this configuration that we've got active. Then let's just change the length to 71.5 millimeters and then you can press. Okay. Now we should have a longer axle like this. And if you go back to the Configuration Manager, you can see we've got three different configurations. We've got the short three, we've got the longer six, and then we've got the longest one, the one we just added, the nine. The three and the nine are gray in color and the sixth is black. Then you can just press Save and that part is complete. A very simple part of that in the next video will be making the longer pushing. 22. Making the Large Bush Part: The next Lego bit that we're going to make is the large bush. And this is a fairly simple model. So let's start a new part and let's start a sketch on the top plane. First, I'm going to get the circle tool, draw a circle at the origin and make that 5.7 millimeters diameter. Then let's do a mid-plane extrude and extrude this 5.1. This is gonna be the center of the bush, and we'll call that feature and middle body. Then I'm going to add those wider rims on each end. So I'm going to start a sketch on either end, face, the circle tool and draw a circle that's coincident to that circle we've just made. The diameter of this is a little bit wider, so at 7.4 millimeters. And then let's do a blind extrude just in one direction going outwards, that's worn 0.4 millimeters thick. Then I'm going to call the outer rim and we need one on the other side as well. So we can mirror this. I'm going to select the outer room feature. I'm going to select the plane that goes down the middle of the model. So that's the top plane. And then I'm going to press mirror. You could also make this whole section with a revolve boss base feature if you prefer. That's the general overall shape. What we're going to do now is cut out the cross through the middle. I'm going to start sketch on the top plane. You could also start on one of the interfaces. And we're going to draw the actual shape that we've done quite a few times now. Get the circle tool, draw a circle at the origin, make that 4.8 millimeters diameter. And then get the center rectangle tool and draw to censor rectangles. Make them both the same width, which is 1.8 millimeters. Then set the length of them by attaching them to the end of that circle using tangent relations. When you've got that profile, we can do an extruded cut through all both. Remember, we need to select all five of those areas in the actual shape. On the preview we're cutting through like that. Then let's call that feature axial cuts. Next up, we'll cut the slot that goes through the middle. So we can either start on the front plane or the right plane. Let's start a sketch there. Guess center point slot tool. I'm going to start at the origin, go up like this. And then for the size is one millimeter thick, the length of it is 4.8. I'm going to dimension to each n by holding down shift. So we can dimension to that, OK? And it should look something like that. You can then do an extruded cut through all both. This just gives a bit of flexibility to the bush to allow you to fit the axial part in properly. Let's call that feature slot cut. Then the final thing we're going to do is just cut away that scalloped circular car at the top. Only one end of the Bush has these cuts. I'm going to start a sketch on one of the n faces. Either one, it doesn't matter. I'm going to go normal too. These curves are a little bit tricky to measure in real life, but I measured the shortest distance between the curves. First, let's draw a circle at the origin. And the size of that is 6.4, and that represents the shortest distance between those circular cards. We've then got some smaller circular sections that we need to cut out from the outer rim. So firstly, we're going to use a central line to draw exactly where we want these cuts. Select a center line by using the drop-down on the line tool starting from the origin. And let's go up and write at about 45 degrees. Then Get Smart Dimension. And let's just add, as I mentioned here, to make this line 45 degrees. We'll then get the circle tool and we'll draw a circle at the end of that center line, somewhere around here. We can make it any size, something roughly like this. Then what we'll do is select that circle, hold down control, and also select that first largest circle that we just drew. And then make those two circles tangent. That means the two circles are exactly touching. We're gonna cut away this overlapping area here. First though, we need to figure out how large this outer circle needs to be. And to do that, I measured the curl across the outside in between here and here on the real model. And that should be 2.3 millimeters. I'm going to get the point tool and I'm going to add a point on that circle, which is also coincident with that main outer circle. We want to add these points where the sketch circle crosses the main outer circle. You should just be able to hover over the intersection and add the point directly. And you'll see these two relations symbols that indicate where at the intersection of those two circles. But if you're having trouble, you can just add the point to one of the circles. Say for example here. Now that point is fixed to that sketch circle. We can move it anywhere around the circle, but we can't move it off the circle. Then let's select that point, hold down control, and also select that main outer circle. We can then add another coincident relation. This point is now coincident with both circles. The only position it can be is where those two circles cross. Now we just need to set distance between those two points and that is 2.3 millimeters. Get the smart dimension tool and just add that distance. Make sure you get the diagonal distance. You might just have to move your mouse around a little bit before you place the dimension. Then you should be fully defined, something like this. We're just going to cut away that little semicircular section. And we're going to do the same four times around. To add the remaining three circles, we can use a circular sketch pattern. First I'm going to select that smaller circle we drink. And then I'm gonna go to the Sketch tab and I'm going to choose circular sketch pattern. This is underneath a linear sketch pattern, so you'll have to click the drop-down there. Now hopefully you'll get a preview like this where everything looks correct already. But if yours looks different, just make sure you have the settings. We want a pattern for instances. It should be equal spacing 360 degrees. And then the center point of the pattern is the center of the main circular body. So that should be lined up with the origin. If yours looks different than clicking this top box and press clear selections. And then just choose the origin or the center point of that large circle. Then press Okay, and that circular pattern around. So we've got four of them. Now if you find that your pattern isn't fully defined like this, you can just drag it around and then add in some more relations. First thing I'm going to drag that center point of the parts and back to the origin. If you find that you still not fully defined, you can try adding a tangent relation between one of the small circles and that large center circle. And you might just need to add one more as well like this, and that should fully define your sketch. Now we're going to cut away those small circles. So I'm going to get a Features extruded car. For the selected contours, I'm going to choose the overlapping circular area. So you can just click on the area or you can click on the entire circle and that will select the entire entity. Then let's cut downwards just through that top rim. I'm just going to cut down 1.4, which is the thickness of that top bring the top should be sort of scallop like that. And I'm going to call that scallop car. This part is now finished so you can save it. I'm going to call mine large bush 30465. In the next video, we'll make the first year that actually drives the helicopters rotors. 23. Making the Bevel Gear: We're now going to model up the first year. It might look like quite complex part, especially once we start modelling, it is not too bad. Let's start a new part and start sketch on the top plane will get the circle tool. And we're just draw the circular body of the gear first. This should be 7.7 millimeters diameter. Then let's do a mid-plane extrude, and we'll extrude it eight millimeters. Then let's call that something like gear body. Now we're going to draw a single one of the gears teeth, and then later on we'll pattern this around. Let's start a sketch on the top lane. Go Normal To get a sense of rectangle tool. Draw a rectangle fixed to the origin, and this is going to represent one of the teeth. This should be 1.5 millimeters wide and the total height of it is 13.4 millimeters. But we actually only want to extrude that top section. Before we extrude. Let's select this outer circular face and press convert entities. That now adds that circle into the sketch. We can now just extrude that top section. Go to the Features tab and choose extruded boss base. Then for the selected contours, Let's just choose that top section. Then we can do a mid-plane extrude three millimeters. So it's just the thicker part of the gear in the middle. And I'm going to rename that feature as tooth middle. Next we'll do a similar thing for the outer part of the tooth. Start a sketch on the top plane, get a sensor rectangle again, and draw another rectangle at the origin. It's the same thickness as the first tooth. We can link it to the outside there. But the height of it is a little bit less. This one is only 12.6. Again, we'll select that circular edge and we'll convert it. And then we'll do an extruded boss base and we'll just extrude this top section. This time we're going to extrude the full-width, so it's eight millimeters mid-plane. Let's call that feature something like tooth outer. You should now have something roughly like this. And next up we're going to angle off the outside edges of the tooth. We can do this using a chamfer. Let's select the chamfer tool. This is underneath the fillet tool. So go to the Features tab, click on the drop-down underneath filler and then 2D chamfer. Make sure that you're on this first option. This is called an angle distance chamfer. And then set the distance as 1.5 millimeters and set the angle is 45 degrees. Then we can just select this edge on the front and the same one on the back. We've angled off those teeth. Next that we need to add a few more smaller chamfers. So again, select the chamfer tool. These ones are 0.5 in size and they're also 45 degrees. We can then select four edges. So it's these two on the front and then the same two on the back. We've now created one of the teeth that we need. We can now use a circular pattern to pattern this all the way around again. To do this first I'm going to select everything we want a pattern. It's the tooth, middle tooth outer, and then the two chamfer features. You should have four items selected there. And then we can select the circular pattern. This is on the Features tab, and it's underneath the linear pattern. So click on the dropdown and choose circular pattern. Over here in the property manager on the left. For the features and faces, we are going to have those four items selected. The tooth middle to the router and the two chamfers. For the instances we should have 12, That's just the number of items we're going to pass in. And then we should have 360 degrees and we should have equal spacing. Then we need to choose a circular face or an access to pattern around clicking this box on the top, and then just choose the circular outer face of the main gear body. Now you should see on the preview that we've got 12 instances there. You can adjust the instances here if you need to, but let's say it to 12 and press. Okay. Now we've added all of those teeth to the gear. You should have something like this. This is pretty much our gear shape. The only thing we've got to do now is cut out that actual hole in the middle. To do this, Let's start sketch on the top plane. And let's draw that usual actual shape that we've done loads of times. Now, let's draw a circle in the middle, set that to 4.8 millimeters. Get the center rectangle tool, draw those two center rectangles, make those both 1.8 millimeters wide, and then set those so that they're tangent with that circle. We can then do an extruded cut to cut out that cross shape. We can do through all both. So it goes all the way through the model. Then finally, let's rename that feature as axial cut. So you should have something like this. This is a representation of the gear part. Then to finish off, we can change the appearance and make it a dark gray. Then I'm gonna save that. And I'm going to call it bevel gear because the edges are beveled or angled 12 tooth. So bevel gear 12230465. This part is now finished. In the next video, we'll be putting all these parts together in stage six. 24. Stage 6: Adding the Tail Rotor Transmission: Stage six, Let's go. So before we start adding to the main assembly, Let's make sure we've got everything open. I've got the main assembly. I've also got those three new parts, the large bush, the longer axle, and the bevel gear. Before we start adding to the main assembly, we're gonna make that small six sub-assembly. Let's go to the axial and let's go to File, make assembly from part. Then just choose the axial and we'll insert it fixed to the origin. This should be the axial That's nine long. If you've got a smaller one, you might just need to click on it and choose the nine long configuration. Then let's insert the two remaining parts. So go to Insert Components, insert the bevel gear and you might need to spin it around. Also insert the large bush and you might need to spin that as well. Then let's add our mates. I'm going to zoom in a little bit and I'm going to select a circular face inside the bevel gear. Also circular face on the outside edge of the axon. I'm going to make those concentric. And I'm gonna lock the rotation by expanding the mate, right-clicking on that concentric mate and pressing Lock rotation. Then if we look at the instructions, the end of the bevel gear is lined up with the end of the axon. So let's add a coincident mate between those two faces. It should look something like that. Then next that's positioned the bushing. Select a circular face on the bushing. It can be anyone and also select a corresponding circular face on the axle and make those concentric. Now it doesn't matter too much which way you get this round. But technically, according to the instructions, the side of the bush part with the cutout should be on the same side as the gear. If yours is in the opposite direction, you can just right-click on your concentric mate and then press Flip Mate alignment. I'm also going to lock the rotation of that bush by right-clicking on the concentric mate and pressing Lock rotation. Then let's just move the bishop so that H touching the end of the year. To do this, you can just add a coincident mate between the bush. And again, there we have our fully defined assembly that let us save this and call it stage six. Now we cannot the sub-assembly to the main assembly. Let's go back to the main assembly by pressing control and tab. Go to Insert Components and choose that stage six sub assembly. I'm then going to align the axilla up with the holes that go through. I'm going to choose a circular face on that sub-assembly. And then I'm going to choose one of those holes and make those concentric. For this one, we don't need to lock the rotation because we actually want this part to spin. Because that's what drives the rotor blades and the tail rotor. We are going to set the distance though. So I'm gonna select this face and also in the back of the bush and make those coincidence. Then finally to finish off, we just need to add another gear at the back. If we hold down control, we can left-click and drag from an existing part. So let's do that without gear, hold down Control left-click and drag and then release the left-click to place a new gear. Let's select a circular face inside that gear and also a circular face on the axle and make those concentric. Now at this stage just makes sure that your gear is actually properly lined up with your axon. If it is a bit misaligned like this, then you might just need to select a flat face inside the actual hole on the gear and then a corresponding flat face on the axle and just make those parallel. So it should be lined up properly like that. And then finally, let's just select this N face of the gear and also the interface of the axial. And make those coincidence. We can see we've got a small gap there that doesn't really matter at this stage, just gives a bit of clearance to allow the axle to spin around. And if we zoom out, we can see this is basically the driveshaft that will run the tale writer. Stage six is now complete so you can save your assembly. In the next section, we'll be moving on to Stage seven, which only has one new part. 25. Creating the Two Block with Axle Holes: Now onto stage seven, and we only actually need one new part for this is a short block that's too long and its got two actual holes in it. This is a very quick part to make an only actually need worn feature. Let's start an IPO and start a sketch on the front plane. Select the slot tool and draw a center point slot from the origin going outwards like this. Then the size of this is 7.4 high and across the outside it's 15.4. Now we just need to draw the axial whole profile that we've already done loads of times. Although there are two, we can just draw one side and then we can mirror it to the other side. Start off with the circle tool, draw a circle that's 4.8 diameter. Then get the sensor rectangle tool and draw those two center rectangle's. Make those 1.8 wide and both the same width. Then add that tangent relation to set the length of both of them. Then we just need to copy that same profile onto the other side. To do this first, we will draw a center line. So select the center line from underneath the drop-down of the line tool and just draw a center line from the origin, going directly vertically upwards. Then select those items so we can select the circle, hold on control, and also select both of the rectangles. You can right-click on one of the lines in the rectangle and press Select chain, and this will select the entire rectangle. You don't have to select the lines one-by-one. Then let's also select the center line. Now because we've only got one center line selected, if we press Mirror entities on the sketch tab, it will automatically mirror everything about that center line. This only happens when you've only got one center line selected. And it should automatically mirror everything like this. If you have any problems with that, you can choose the Mirror Entities tool first. Then you can select what you want to mirror. So it's the circle and the two rectangles. And then you can choose where you want to mirror it, which is that center line. So now we've got the profile that we need before we extrude this, I'm just going to check that between those two holes, we've got that correct eight millimeter spacing that we had for the other paths. If I quickly use smart dimension, we can see, yes, we do have eight millimeters there. Now let's just do a mid-plane extrude. So I'm gonna go to Features. I'm gonna choose mid-plane. And this is four millimeters exactly. Then for the selected contours, Let's choose everywhere apart from those actual curves. It's the large main area. And then it's those corners around the cross. And then also those small wedge shapes at the end of each arm of the cross. Then it's just the same on this side. So it's the corner sections. And then the small wedges, those two for each arm. So there should be eight in total. When you've got all of those, make sure you're on a plane four millimeters and press okay, this part is now finished. So let's change the color to a dark gray. Then let's save the palette. And I'm going to call it to beam with axial holes. And then 30465 and press Save. In the next video, we'll be making Stage seven using this part and some existing parts. 26. Stage 7: Building Up the Main Rotor Hub: We're now on to Stage seven. So firstly, we're going to make this small sub-assembly, and then we're going to add that to the main assembly. Before we start, make sure you've got the main assembly open. I've also got opened the axial part and the two beam with axial halls part that we made in the last video. And I'm going to start with the actual part. So I'm going to open one of the axial parts. I'm gonna go to File make assembly from part. I'm going to pin the insert menu open. And first I'm going to insert an axle just fixed to the origin. So choose the power and then press the green tick at the top-left to do that. Then I'm going to insert another axial. This time I'm not going to click the green tech. I'm just going to left-click somewhere in the graphics area that will insert another accident that isn't fixed. And then I'm going to insert one of those new two-block with actual whole pot. And then I can mirror the second one over because it's on the other side of the assembly. For your axons, make sure that they're the three long configuration. You might just need to click on them and choose three long from the drop-down menu. Now let's start to add our mate. I'm going to select circular face and a corresponding circular face. I'm gonna make those concentric. And I'm gonna do the same with this one at the back. And then I'm going to lock the rotation of both of those. So I'm gonna expand the Mate, right-click on each concentric may in turn and press the lock rotation. Next I'm going to make the two ends of the axial lined up. Let's select both of those faces and just make those coincident. We can now move that to block in and out, and we want to make it so the inside face of it is at the center of the assembly. It's not quite in the middle, but just off to one side exactly. So let's select this inside face and then also select the plane that goes down the middle of the assembly and then add a coincident mate. We are now fully defined, but we're still missing that tubing part on the other side. So we can mirror this over. To do this, I'm going to select the part. I'm also going to select the plane down the middle of the assembly. And then I'm gonna mirror. To find the mirror command, we need to go to the Assembly tab. Click on the drop-down under linear component pattern. And at the bottom now you should see mirror components. Then you can choose the next arrow. And we can see on the preview that all looks correct. So we can press OK. And there we have created that serve assembly for Stage seven. We can save this as Stage seven like our helicopter. Now let's go back to our main assembly and let's insert this new server assembly. Use Control tab to go to the main assembly and then go to Assembly, insert components, and choose that stage seven assembly that we just made. You might need to rotate it around to the correct orientation. We want to fix it up here somewhere. So what I'm gonna do is select a circular face inside the actual hole and also select the corresponding face on the axle. I've made those concentric. I'm gonna lock the rotation. You can actually do that from the smaller pop-up menu that comes up. If you don't see that, you can also scroll to the bottom and you can do it in the usual way by expanding them eight, right-clicking on the mate and choosing lock rotation. Now to finish off, we're just going to put that new stage seven sub-assembly exactly in the middle of our assembly. So perhaps we could just make the faces of the corresponding parts. But instead I'm gonna use the planes just to make sure that the sub-assemblies right at the middle of the model. To do this, I'm gonna find the assembly in the street. She'll be the latest one. I'm going to expand that assembly and then I'm going to choose the plane that goes down the middle. Then I'm also going to choose the plane that goes down the middle of the main assembly. And then I'm going to make those coincidence. Now we've finished for Stage seven, so you can save your assembly. That was quite a simple stage. They're in the next video we'll go into a stage eight. We don't actually need to make any new parts for that because we've already got everything we need. 27. Stage 8: Adding the Helicopter's Nose Section: Carrying on from Stage seven, we don't actually need any new parts, so we can go directly onto stage eight. We are going to create the small sub-assembly for stage eight. We probably don't really need to do it because it's only two parts. But we're gonna stick with the same process that we've used so far. Before we make the assembly, Let's make sure we've got the appropriate parts open. We can open the axial part. You can click on it in the assembly and press open part. And then you can press Control Tab to go back to the main assembly. And then next we need to open the small brush. You can also click on this in the assembly and press open part. We can now start the new assembly so we can go to file, make assembly from part. We can choose the axial and we can insert that fixed to the origin. Makes sure that you're using the three long axial. So you might need to click on it and choose the three long configuration. Then will also insert the small bush part. We only need those two parts. We can now make them directly together. So I'm gonna get a circular face from each part and make those concentric. And I'm going to lock the rotation. I press the lock rotation but are there but I think I actually pressed it twice. I'm just going to check that that's locked. And if we expand them HCI, we can see it's not locked. I'm going to right-click and press lock rotation. Then for the left, right position of the bush. If we look at the instructions, it's not really clear how far along the axial we should put that bush. Let's look a little bit ahead in the instructions. If we go to the main assembly, we can see that this right angle beam should be in-between the two bushes. So let's measure the length of that and that should give us the spacing for the bushes. You can do this using the measure tool. You can find this on the Evaluate tab. And let's just find out that length is 7.85. Let's go back to our assembly and we can now use this dimension to set the spacing of the bush. We know now that we need a gap 7.85 millimeters between the two bushes. So let's select this face that's also select the plane that goes down the middle of the assembly. And let's set a distance mate. We want 7.85 in total, but we're actually meeting to the center of the assembly. We only actually need half of that amount. To figure this out, we can write in 7.85. And then before you press okay, also write slash two and then press Enter. This will divide by two what we wrote in 7.85 divided by two, which equals 3.9 to five. So we can then press Okay to add that, that assembly is fully defined. We can save that as stage eight. Now let's go back to our main assembly and insert that sub assembly. It go to Assembly, insert components, and choose that stage eight sub assembly. I'm going to spin it around like this, and then I'm going to fix it in place using concentric mates. Also going to lock the rotation. We probably don't need to do it for this one, but I'm just gonna do it for completeness. Then for the left, right position, I'm gonna make this outer face of the beam coincident with this interface of the bush. Now we know that it's exactly in the middle of the model because we measured that middle section already. Then to finish off, we just need to add warm or bush to the other side. Let's insert another one of the bush parts so you can hold down Control, left-click and drag from an existing bush part and then release the left mouse button to insert a new one. We can then make that in position using concentric mates. We can lock the rotation. Then I'm just going to drag it out. So I've got enough space to add a coincident mate in there. And we're now complete with stage eight, very quick stage they're in. The next video will be modelling up another part which forms the outer frame of the cockpit. Then we'll be adding that in stage nine. 28. Create the Right Angle with Curve Part: Welcome to stage nine. And for this one, we need to make one knee par, and it's pretty similar to this right angle beam that we've already made, but it's got an extra curved edge along the top. We can use this existing part and we can make some changes to that from within your assembly. Let's open that right angle being part. You can also just open it directly from wherever you've saved it. Now let's save this as a copy and make some changes to it. So go to File Save As, choose save as copy and open. And if you don't get this pop-up, you can also choose save as copy and open from down here on the left. Now let's rename it. So it's actually five by three long. So let us say right angle being five by three. And then I'm going to also say with curve. So it's right angle beam width curve five by three. So we'll save as copy and open and press Save. And then you can close the original document if you need to. First, I'm going to drag up to the very first feature. I'm going to edit the sketch that's underneath it. And I'm gonna change it from four-by-two to five by three. Firstly, we need five holes along the bottom. So I'm going to double-click on the number four for the pattern, and I'm gonna change that to five. And that should add a fifth circle here on the right. However, if we look at the sketch, we can see that the vertical section is still linked to that fourth hole. So let's zoom in. Let's delete those coincident relations. There's actually three of them. We don't know which one is the correct one, so let's just delete all of them. Then when we no longer have those relations, you should be able to drag that slot out to the right-hand circle. You probably have to drag them out one by one. So I'm gonna start with the lower one. And then I'm also going to add that vertical upright one. You should be again fully defined with five circles along the bottom. We also need to make that vertical section three high. But we didn't actually use a pattern for that because there was any two holes in it. So instead, let's double-click on the dimension here will change it from eight to 16. We know that the spacing between holes is eight millimeters. If we add another eight millimeters on, that will give us space to add that third hole. And then let's just add an extra circle using the circle tool and we'll make it the same diameter as the others by using an equal relation. You can then exit the sketch and we should have something like this. Now if we look at the actual part is not as thick as this, so we now need to edit the feature. Let's edit that being feature. And let's change the thickness down to four millimeters, but keep it as a mid-plane. We also have an axial or a cross shape on this right-hand hole and the top hole, clicking selected contours and then choose those two circles. So it's the one in the right-hand corner and the one at the very top. Then when you exit the feature, we should have something like this. The holes on the left, right, and top are all filled in. Now we can add those axial cuts. So let's drag down below the next feature. So we've got the first one correctly, but we need to add two more days. Let's edit the axial cut. Now for this lower coat, we can actually just mirror the one on the leftover because they're both the same but just reversed. Let's get the center line tool. And let's draw a center line going up from that middle circle, going directly vertically upwards. We can then use this for the mirror. Then I'm going to drag a box around everything here on the left, except for those two horizontal lines. So it's everything else here on the left. We don't need to select those lines because they already go over to the other side, so we don't need to mirror them. Then I'm going to choose Mirror entities from the sketch tab. For the mirror about point. I'm going to choose that new vertical center line that we just made. For the preview. You should have something like this. So we've mirrored everything apart from those horizontal long lines. Then let's press Okay to add those. And then we can just drag those horizontal long lines out so they touch that large circle like this. And then we have the correct profile for us to cut out. And that was a very easy way to add that second sketch. Now we just need to draw a similar profile here at the top. Let's just do this one manually. So let's get the circle tool. We'll draw a circle out that's 4.8. Then let's use the center rectangle tool to add our two rectangles, will make those the same width and will make them 1.8. And then we'll make the ends of them tangent with the ends of that 4.8 circle. And then if you remember, we had to offset the second circle by 1.3. I'm going to select that circular edge and offset that 1.3 millimeters like this. And then also select this one and offset it. And just make sure that both of the lines or solid lines, so you don't have any of those construction geometry options selected. Then next, if you remember, we offset these outer lines by one millimeter. So let's select this one and offset it inwards one millimeter. Then also this one on the other side, offset at inwards one millimeter. Then finally, we just need to add those small lines here and here. We can then exit that sketch and we've got everything we need. You'll probably find that we're still just cutting out that area on the left. So now we need to edit the feature. Then we need to go into the selected contours box and we need to choose those new profiles to be. Here in the corner is all those areas of the cross. Then it's that little rectangular area and also that wedge-shaped area. Then also those two little tiny wedges. Then at the top here is the same thing. It's the five areas of the cross. It's the little rectangle. It's the two tiny wedges. And then it's the larger wedge. Then press okay, and now we've cut out those three axial cuts. And it should look something like this. Next we can drag down below the next feature that's the whole surround. So when you do that, you'll probably find they've got some kind of error on the sketch. That's just because we've changed the number of holes in the model. Let's click on that feature and edit the sketch underneath it. We can just delete that extra circle that we don't need. And then let's just add in this fourth one here. Let's just select that circular face and let's offset 0.7 like this. And then press Okay, and we've now cut out all of those room cuts correctly. Now let's go down below the cavity cut. So we're cutting out these two cavities on the left correctly, but we still have an error on the sketch. We're also missing the cavity on the right. Let's edit the sketch and we can see immediately that there's a lot of areas in this sketch. So it's probably easiest just to completely delete everything in this sketch. Let's press Control a and then press Delete. So starting again from scratch. Firstly, if you remember, we offset the circular lines of the existing whole ribs. So let's select the outer edges of all four of these holes. Let's convert them first and then select those for converted circles. And then let's offset those circles. We just converted them first because sometimes offsetting directly like this doesn't quite work when you've got multiple edges selected. Then let's offset 0.55 millimeters. And before you press OK, we want the base geometry to be construction and we want the offset geometry to be solid. Then we can offset the large outer lines. From here. This top one is one millimeter inwards, same with the bottom, 11 millimeter upwards. Then on the right here is one millimeter as well. But on the inside here on the left is actually a little bit bigger to allow for the cavity in the corner. So let's select this one and offset that 1.2. Then let's zoom in. Let's select this curved edge and convert it. Then just drag the edge of that curve around until it touches this other straight line, something like this. Then also drag down the straight line on the left so it touches that new curve. You might have to zoom in to get this exactly right. The end of the vertical line, it should be exactly touching that curved line. It looks like a really small gap there that we're going to cut out. But actually once we add the fillets in, this will add more material. Let's now exit that sketch and you might get some warnings or some areas like this. You can just ignore them at this stage. Then we can edit the cavity cut feature and we can choose which areas we want to cut out. Here in selected contours. Let's just choose those three areas. So it's these two on the left and then the vertical one on the right. And we're still cutting down blind three millimeters. So you don't need to change that. Then just press Okay. And we've got those cavity curves like this. Next we can drag down again for the fellows and you probably have to edit this feature, click on it and press Edit Feature. And I'm just going to clear the entire selection. And then I'm going to re-add in those 12 pillars. We've got four inside here, for inside here. Then also for inside here on the right. We can see by adding that felt that it gives a bit more material there on the right where that really small section was. Now before we drag down below the mirror feature, there's actually an extra curved arm at the top here. To draw this, Let's start a sketch on the front plane. And we'll use the spline for this because it's not actually a constant curve all the way round. Get this blind tool, which is this one. We're going to start at the midpoint here on the left, and then just go directly up to the midpoint here on the right. We don't need any extra points in this plane. And it should look like a straight line. Initially. We now have this spline and if you click on it, you should be able to see these handles. And we can move it around to roughly the correct position, which is like this. Now if you don't see those handles, you can just go into your options, then use the search function within the options and just type in spline. And you should be able to see an option that allows you to turn on those spline handles. Now for this curve, we could just eyeball it and get something that's pretty similar. But actually we can add some tangent relations, which should get it exactly right. Before we add these, we're going to add some sense of lines to help with adding the relations. Get the center line. And then here on the right, Let's draw one from the endpoint of the spline going outwards horizontally. And then here on the left, Let's draw another one from the end of the spline, but going downwards vertically. The center line should start from the end points of this flying. We can then select the spline and select one of the center lines and add a tangent relation. Then do the same thing on the other end. That will just mean that the spline joins the endpoint or the correct curve. Next step we're going to offset this spline inwards. So we've got the correct curve of the area we want to extrude. I'm going to select the spline. I'm going to offset and the thickness of it is 3.7. And make sure you don't have any construction geometry options selected. We want both of the lines, the base and the offset one to be solid lines. Now we've got two lines that follow the same curve around like this. Before we can extrude this, we just need to add in some extra lines at each end to close the profile. So zoom in a bit. Let's choose this curved edge and this straight edge and press convert entities. Then let's do the same on the other end. So zoom in, select the curved edge and a straight edge and press convert entities. We're now going to extrude the inside section. I go to Features extruded boss base in the selected contours. I'm gonna choose that middle section. And then we can do a mid-plane extrude and it's the same thickness as the rest of it, so it's four millimeters. Now if you have problems making this, if you find you don't get your preview like this, just make sure you have thin feature on Chet. Sometimes this feature is automatically selected when you've got a sketch with overlapping lines like this. We don't want thin feature, we just want a normal extrude. Then when all is good press. Okay, and we've added that extra section at the top. And then I'm going to rename that as something like curve. Now we just need to cut out the cavity inside that top curve. To do this, Let's start sketch on the outer face. Then I'm going to select the inside curve. And I'm going to offset this 0.8 millimeters. That's the wool things. Then let's also do the same with the outer curves. So select the curve, press offset entities and then offset inwards 0.8. We also need to add just two more lines. So I'm going to select this curve and press Convert. And then they're going to drag the end point of the converted lying around. So it goes all the way around like this. Then let's do the same on the other end. So slightly curved face on the end, press convert entities and then just drag the line around so it's a little bit longer like this. Now we just need to extend the curve of that inner spline so it touches that new line that we just drew. You can do this using the trim tool. The trim tool actually allows you to extend items as well as trim them. Let's choose Trim Entities. Make sure you're on the Power Trim option. The first option to trim all you need to do is hover over the line you want. Hold down the left mouse button and then just move the mouse to the line you want to extend two. And let's do the same. On the other hand, click on the line you want to extend and hold down the left mouse button and then just move the mouse over the line you want to extend to. We can then cut out this middle section. So let's go to Features extruded cut. And it's just a blind cut, 1.4 millimeters deep. For the selected contours, choose the intersection. And again, make sure you don't have thin feature selected. You might need to uncheck that option. We're making a cut at something like this. And let's call that curve cut. Now let's drag down below our mirror feature. So we've now got the fillet on the other side. We also want that cavity cut on the other side. Let's edit that mirror feature. Then clicking the features to mirror box. And let's also add a cavity cut. You can just click on it in the graphics area. Or you can expand the second feature tree and you can choose the curb cut feature there. Then the final thing to do is just add in the remaining fellows. Let's drag down below that final feature. And then we've only got the fillets on the left cell. Let's edit that feature. Let's add the remaining eight fillers. There's four here. And as we add the one in the top right corner, it gives even more material there. Then there's a final four up here at the top. You should have 12 in total. And you can see now we've got that extra material there in the corner. You can then save this part. And in the next video, we'll complete stage nine by adding this to the main assembly. 29. Stage 9: Create the Cockpit Side: Welcome to stage nine. This is a very quick video. We only need to add one single part. That's the part that we just made, that right angle with a curved edge. Open the main assembly. Also open that right angle beam with curved part that we just made. And then from within the main assembly, let's go to assembly, insert components. Let's choose that right angle beam with curved part. Let's insert it and spin it round to the correct orientation. We can then zoom in, I guess, circular edge inside the actual hole and also circular edge on the axle. And we can make those concentric. We can lock the rotation from the pop-up menu. Remember you can also go down to the mix at the bottom of the part street and you can lock the rotation there. We can then just move it into the correct position. Let's select this inside face and also the outside face of this bush part. And let's make those coincident. That's all there is to it probably one of the simplest assembly steps that we've done so far. So you can save your assembly. In the next section, we'll be going onto stage ten. And for that we need to make two new parts, but they're pretty similar to things we've already made. 30. Make the Three-Long Cross Block Part: Welcome to stage ten. For this one, we've got to make two new parts. You've got to make across block that's three long. And we've also got to make an axle with a pin connector in the middle. We'll start off with that longer across block. And if we look at it, we've actually already made something very similar. We've made one with two holes instead of three. Let's open that existing parts from within your assembly. You can click on the part and press Open, or you can just open the part directly. The part that we're now going to make his very similar, except it's got two holes here on the right instead of one. Let's save this and make some changes to it. Go to File, Save As, and then choose save as copy and open. And remember, if you don't get this part, but we can't just choose it from the options down here on the left. And let's change the name to something like cross block three long. Press save as copy and open, and then press Save. And then you can close the original document if you like. Now let's have a quick look how we could modify this. First we have the pin part and then we added those two ideas. Then we added the middle rib and we cut out the actual home. Perhaps we could just use this finished part and we could just add on an extra hole on the end. But having to think about it, it might be easier if we extend those ideas and then we can add the extra hole, but it was still have all the correct rib and everything in the middle. Let's edit this sketch underneath the side here feature. Let's change this 15.4 so we can fit an extra hole in there. We know that the holes are always spaced eight millimeters apart. So let's just double-click on this 15.4 and add eight millimeters. So you can just write plus eight millimeters. That should be 23.4 in total. We can then press OK and exit that sketch. And then we can drag down to at the second warning. And then we can keep going down all the way to the bottom. And we've pretty much got everything we need that we just need to add that second pinhole in. To do this, I'm going to go back above the pin rib because that rim will apply to both holes. Then we can start a new sketch on the plane that goes down the middle of the path. So for me this is the front plane. I'm going to get the circle tool. I'm just going to draw a circle. There should be eight millimeters from the original pinhole. We also need a second circle for the hole that goes through the middle. So firstly, let's make this larger one tangent with the outer edge. You might also just need to make sure that the center of it is lined up horizontally with the center of the original circle like this. That should fully define that large outer circle. Then the smaller inner one should be the same diameter as the hole through the pin on the left. You can select both of those edges and make them equal. And you should have something like this. We can then do an extruded boss base mid-plane. And let's get the full width. So 7.4 millimeters. That takes us out to the side like this. And that's cool, that second pin body. Then we also need to cut that hole through the middle. So I'm going to start another sketch on the front plane. I'm just going to select inside that face there and press convert entities. So that will make the outside of the face we've selected, which is the circle we want into a new circle. We can then use an extruded cut and we can go through all to cut out circle. And let's just call out something like second pinhole. So by making it this way, it means we've automatically got that correct cavity area in-between the two pinholes. We can then drag down below the pin room feature. So we've cut that out with the first hole. We also need it from the second one. Let's edit the sketch underneath that feature. Let's add another circle that's the same size as the first one, but let's lined up with the second panel. You can just select them both and make them equal like this, and then exit the sketch and you should cut that rim cut correctly from both of the holes. Now before we go down to the mirror, I'm just going to round off the inside edges of this cavity here. I'm going to get the fillet tool and I'm going to set a fill at this 0.5 and I'm going to add it to all four of those edges inside the cavity. We can then drag down below the mirror feature. Let's just edit that feature. And we'll add in that fillet that we just created here in features to mirror. Let's just zoom in and select that fillet. And then we have our finished part like this. And let's change the color to that lime green. And I'm just going to edit the color to more closely match the real world. Then you can save the part. So that's that one finished in the next video will be making the axle with a pinhole in the middle. And then after that we'll be making stage ten. 31. Create the Axle with Bore Part: Welcome back. The next part that we need for stage ten is an axon with a ball or a hole in the middle. We've made a part that's pretty similar to this already there. This one is a friction pin with a bore. Let's open this part and make some changes to it. We want to make something very similar to this, but instead of the pins on the side, we want an actual. First. Let's save this part as a copy, go to File Save As, and then choose save as copy and open. Let's call this part acts or with Bohr and then press save as copy and open. You can close the original part. Now let's make some changes to this. So I'm going to drag up all the way to the first feature, the pin. I'm going to edit the sketch underneath that feature. We want to change it from a round pin to that cross shape, the actual shape. Let's change that circle to 4.8 standard size that we've been using. Let's also use to censor rectangles. We'll set them the same width, 1.8 millimeters. And then we'll fix the length of them to the outside of that 4.8 circle. Now when you exit the sketch, you'll probably get an error because we've got overlapping lines in the sketch now, you can ignore this error and just rebuild anyway. And if you get a secondary like this, you can ignore that as well. And if we click on the feature here, we can see we get the error. The sketch has self-intersecting contours. We now need to edit the feature itself. So click on the pin and press Edit Feature. And then hearing the selected contours, Let's zoom in and let's choose those five areas of the cross-shaped axil. It's the middle, and then the four outer crosses. We want to stay as a mid-plane extrude. But for the length is slightly longer, it's going to be 23.4 millimeters and then press OK. Next we can drag down and we can keep that middle the same. Then for the next four features, we don't need any of these because these are just for the pin. This is the outer rim, the bore, the slot, and the mirror. We can delete all for those. They're all actually dependent on the outer rim feature. If you just delete that first outer room feature, it should automatically delete the other three features as well. Then you might also just have to delete the sketch. And then we can drag down again. We can add that middle body and the middle ball, which is the hole through the middle, we cannot the rim cut. And then finally we can mirror it over to the other side. That's almost all that we need. We'll just add some fillets, get the fillet tool, and we'll add a 0.5 millimeter fillet, these four edges on the end. And then the same for riches on the other end like this. That's all of the modelling. Now we can change the color. So I'm gonna go to a parent says this isn't quite a black, it's more of a dark gray. But remember, we've already used dark gray in place of black. I'm going to select a light gray. And that looks correct. Then you can save your part. In the next video, we'll use these to new parts with the rest of the parts and will complete stage ten. 32. Stage 10: Make the Main Rotor Hub Section: We can now make stage 10 first. We're gonna make this smaller sub stage. First, make sure you've got everything that you need open. So we've got the axial, we've got the cross block that's three long. We've got the friction pen, we've got the small Bush. We've got the axle with Bohr, and then we've got the two beam with axial holes. Now it doesn't really matter too much which you start with. I'm going to start with this one. Just because it's right in the middle of the assembler. I'm gonna go to File make assembly from part. I'm gonna pin the insert menu open because we've got quite a few parts to insert. First I'm going to insert that cross block three long. I'm gonna rotate it around to the correct orientation like this. Then I'm going to insert all of the other components at this stage. Firstly, it's the small axial there. Next It's the friction pen. I'm going to insert that new axle with board that we just made. Also the small brush. Then finally I'm going to insert that to beam with axial holes. Then you can close the insert components menu. Now before I actually made anything, I'm gonna check that first component is lined up properly with the assembly planes. I'm going to go to a top view and I'm going to hover over the plains in the assembly. And we can see that it's offset from the assembly planes. So to fix this again, to right-click on the part in the street and then press float. We can now move it around to wherever we want. I'm going to expand that first part across block part and find the plane that goes down the middle, which is this one. And then I'm going to line that up with the assembly plant. Then I'm going to do the same for the remaining two planes. I'm gonna get the front plane here and line it up with this plane in the part. Then I'm also going to get the top plane and line it up with this one. Now that cross block part should be fixed to the assembly in the right position, then it's just a case of meeting all of the other parts in place. I'm going to start off with a small Axel. I'm gonna make that concentric with the hole at the front and I'm going to lock the rotation. I didn't quite lock that one. I think I clicked the button twice, so I'm going to expand the mate and I'm going to lock it here. I'm then going to send to the axial by getting the plane that goes down the middle and aligning that up with a plane that goes down the middle of the assembly. And when we do things like this, you can really see the value of using those mid-plane extrude. Next, we can make the friction pen lined up with the whole. We can lock the rotation and then I can drag it down to the correct place. And I'm gonna make the bottom of the friction pen and the bottom of the beam coincident. Next up we can add that new parts so we can make that concentric with the friction pin on the top and we can lock the rotation. For the height of this top piece. I'm gonna make it so at least two interfaces are both touching, so they're coincident. But if we look at the part, we can now see the pain is sticking out at the top. So this may cause us some issues later on, but for now we'll leave it as it is and we might come back to that later. Next up we can make the bushing place. Let us select the circular face, also a circular face on the axial and make those concentric. And let's lock the rotation. Then let's just make the inside face of the bush and the outside face of the beam. Then finally, let's move the two beam with axial holes into place. I'm going to get the circular face inside here and also on one of the axial connectors. And then I'm going to make those concentric. I'm going to lock the rotation. Then I'm just going to make this outside face and the inside face of the beam. We've almost got that sub stage from stage ten that we need. We just need to mirror over two more components. Let's choose the plane that goes down the middle. For me, this is the right plane. Also select the two beam with axial hole and then the bush part. And then go to assembly, go to the drop-down underneath linear components pattern and choose mirror components. So we've got the right plane selected and we've got those two parts selected. We can then click Next. And we can see on the preview that looks right. So let's press Okay. And those two new parts are added. And there we've got that sub-assembly created there. So let's save this and let's call this stage ten. We can now insert this stage ten to the main assembly. So let's go back to the main assembly. Let's go to Insert Components, find stage ten, and then put it in the assembly somewhere about here. Then to actually meet it in place, let's select this circular face, and let's also select a circular face inside this part. And let's make those concentric. And let's lock the rotation there. And then for the left-right position, Let's just make sure it's in the middle. We could line up the outer face of the bush and this beam. But instead we'll use the planes that go down the middle of the assembly just to make sure it's definitely in the middle. Let's find the plane that goes down the middle of stage ten. And let's line them up with a plane that goes down the middle of the assembly. Like so. Now if we zoom in, we can see we've got a very small gap between these parts that's just due to the tolerance and the way that we've measured these parts, we might be slightly off with measuring them. There we've completed stage ten, so we can now save this. In the next video, we'll move on to Section 11, and we've only got to make one new part for that. And it's pretty similar to things we've already made. 33. Create the Four Beam with Extension Part: We're now onto stage 11. So we've almost finished the first page of the instructions. For this. We've got to make one new part. This is a beam that's for long, that has an extension on it. Now to make this part probably the most similar one that we've made so far is this right angle beam with a curve. So let's open that part and then save it as a copy and make some changes. Let's go to file, save as copy and open. I'm going to name it as something like full beam with extension. And then save as a copy and open. You can close the original file. Now to create the full beam first, let's delete everything we definitely don't need. We don't need this curve on the top, and we also don't need the curve car. But actually if we try to delete the curve, we can see it's got some child features. So if we delete the curve, these features will also be deleted. One of them is the mirror feature. And we actually want to keep the mirror feature because it mirrors the whole surrounds over to the other side. So before we delete this curve feature, Let's first edit the mirror feature. And let's remove that curve cut from the features to mirror. We can then exit that mirror feature. We can now delete that curve feature and the curve cut feature and it won't affect the mirror. You can also delete the underlying sketch that will be leftover afterwards. Now we can start to edit the rest of the part. Let's start off by editing the first feature and editing the sketch underneath it. That's the beam. Now firstly, we only need to be for long. We don't need five holes, we need four. Let's double-click where it says five. Let's change that down to four. We can then delete this vertical section on the right, and we can delete those two extra circles. Then we can drag in the outside of the slot. So it's concentric with this right-hand circle. We should have a full long beam like that. Let's press Okay. If you get any errors, you can just ignore those. And we should have something like this if you drag back to the first feature. However, we've only got one side filled in. We want both sides filled in because there's an axial cut on both sides. We need to edit the beam feature itself. Let's edit the feature. And then in selected contours, Let's just choose this circle on the right-hand side. When you exhale, you should have something like this. It's a full long beam, but it's only got two holes in the middle. Then let's drag down below the actual cup. And we can see this is sort of worked, but we still need to make some changes. So let's edit this sketch underneath this as well. First off, we can delete all of this stuff up here because we don't need this. And now if we look at the remaining sketch, this part where the axial cut on the right is actually in the wrong place, is being mirrored about that third hole as if we've still got five holes in the beam, but we've only got four now, so we need to move that mirror point somewhere to the left. What we can do instead of deleting this and redrawing all, we can actually just move that mirror point. Click on the bottom end of the center line. And there should be a few coincident relations. You can delete both of those relations, and then we should be able to drag that center line around. And that will move where the mirrored part of the sketches. To get to the correct place. Let us drag it to the left a little bit. And then you can drag down and just hover over the midpoint of that bottom line. When you get to about the mid point, you should see a midpoint relation appear. You can then release the mouse button and we should lock that sense alone in the correct place in the middle. You should see your sketches now fully defined. We can then press Exit Sketch, and that should work correctly. You should have a feature something like this. Now if you have some problems at this stage, if yours looks a bit different, you might have to go in and edit the feature itself, and then just edit the selected contours. You might need to choose all the areas we want to cut out correctly. So it's the cross area on both sides. It's also that kind of wedge-shaped. And then it's the little rectangle that joins the two sections together. We should come out with something like this. Next up we want the whole surround. Let's drag down below that feature. And again, we've got a warning on the sketch because we've lost some relations there somewhere. Let's edit the sketch underneath the feature. Just delete all those extra entities that we don't need. We only really need two circles in the middle for those two central holes. Then press Okay, and that whole surround should be created. Next we can drag below the cavity cuts. Now we only need the cavity cut in the middle. So again, let's edit the sketch underneath this cavity cut feature. And we can delete all of this extra stuff up here. We can also delete this stuff on the right here. If you find that your circles become undefined, so if they turn blue, then you can add in some extra dimensions. If you need them. You can then exit the sketch and you see for me that's cut out the correct area. For you. You might just need to go in and edit the feature and choose that central cavity cut. The depth here should be 1.4 millimeters, so it doesn't quite go all the way through. Next, you can go down below the fillet feature. And you'll probably just have to edit this and remove any missing edges there. So we should just have those four edges in the middle. Next we can drag below the mirror and that will add the cavity cut and the whole surround on both sides. And we can go all the way down to the bottom below that final filler. And then we can edit that and we can remove any missing edges. You should just have eight of them, four on each side. We're now almost done. We've just got to add the extension on the right-hand side. Let's start sketch on this outer face. And the extension profile in the middle is just a normal circle. So we'll get the circle tool will draw a circle that's five millimeters diameter. So it's just a little bit larger than the usual 4.8 that we use. Then let's draw a second circle and you can link that to the outside. If you need to set the size for that is 7.4, we can then extrude this profile upwards. But before we do, we need to cut out those scallops on the corners. Now these are pretty similar to that large bush part that we made. If I quickly go back to that part, It's the same sort of cut. So as these corners sections cut away, we can just have a quick look at that sketch to remind ourselves of the dimensions. It's an inner 6.4 millimeter diameter circle. And then there's those four outer circles that I've got a gap that's 2.3 millimeters. Let's go back to that part that we're working on and copy that kind of sketch. First I'm gonna get a center line, going to draw a center line from the middle of the sketch going up and to the right. And I'm gonna make sure that it's at 45 degrees to the vertical. I'm then going to add a circle at the end of that center line. And we also need to add another circle in the middle of the two concentric ones, and that circle is 6.4 millimeters diameter. Then if you remember, we made the outside of this small circle tangent with the 6.4 circle. This means that there are exactly touching each other. Then we added two points on that small circle where it intersects with the outer circle of the par. Get the point tool zoom in a little bit and then just hover over the intersection between the outside of the part and that small circle. Now when you've added those two points, you should be able to drag them only along the outer edge and the circle. If you find that you're missing one of those relations, you can click on the point, hold down control and also select the circle that you're missing and then add a coincident relation. Then let's just get smart dimension and let's set the size across that gap as 2.3 millimeters. That should then fully define your circle. We can then pass in this circle around, so we've got four of them. Let's select the circle, go to the Sketch tab, click on the linear sketch pattern drop-down, and then choose circular sketch pattern. In the settings we want to choose four instances, 360 degrees and equal spacing. If you find that you're patterning around the wrong point like this, what you can do is right-click here in the first box and press clear selections, and then zoom in. And then for the center of the pattern, Let's choose the center point of the axial circle. And you see now we've got the correct preview so we can press Okay. Then if your sketch is still undefined, you can just add some tangent relations between the small circle and the 6.4 circle. You might have to add two of them. And when you're done, your sketch should look something like this. We now need to extrude a certain area here. So let's go to Features extruded boss base. We're doing a blind extrude. It's 3.85 high. Then in the selected contours, we need to choose this inner circle here. And then we need to choose these four outer areas of the circle. Then let's press Okay, and it should look something like this. We can rename that as extension. You can then save this part. The color doesn't need to change. And in the next video, we'll go on to stage 11, and we'll add this part in that. 34. Stage 11: Make the Upper Fuselage Section, and Troubleshooting: Welcome to stage 11. We're now halfway through the stages and we've actually made a lot of the parts that are needed in the latest stages, so they should be a little bit faster. Now this stage appears very simple. There's only one part to add, but actually, we're going to have a look at some troubleshooting and some things that can go wrong when you're working with modular parts like Lego. Before we start, make sure you've got the main assembly open and make sure you've got that for beam extension that we just made open as well. Let's insert that part now. So let's go to assembly, insert components. And we'll choose that full beam with extension. And we'll put it in a position like this. Now, we know it attaches in this place, so I'm going to choose a circular face here on the axle and also inside that hold on the full beam. And I'm going to make those concentric. And I'm gonna lock the rotation. And I'm also just going to bring the part into the correct distance by choosing the inside face here and the outer face here and making those coincident. So at first glance, it looks like our stage is completed. But actually, if we look more closely, we've got some problems. The parts from the different stages don't quite fit together here. And if we look from the side, it's really obvious this axial and this actual hole don't line up. Now some of this might be due to the flexibility of Lego. When you make this in real life, the parts are gonna move around a little bit and maybe bend slightly, and that will allow these small changes to fit together. It might also be due to small differences in measurement. For example, one part could maybe be measured 0.05 millimeters to large. And then over a number of parts, that small difference will add up. But if we look at the side of our assembly here, we can see something obviously isn't quite right. It's not just a small difference there. Let's do a little bit of troubleshooting. Let's get the measure tool from the Evaluate tab and start to try and see what the problem is. We know that the nominal or the usual size between sets of holes should be eight millimeters. That's a pretty standard measurement throughout Lego. Just looking at our assembly, it looks like all of this bit on the left is a little bit too far back or too far to the left as we're looking at it now. So if we try measuring, say from here to here, it's coming up at the bottom as a 16.97 millimeters. Now if we were expecting eight millimeters between holes than we'd expect that to be a multiple of eight. So it should be 16, not 16.9. Maybe we've got some kind of problem with this corner beam pot without diagonal section. If we made that Shorter, who bring everything forward and down a bit. And that seems like it would solve a lot of our problems. So let's open that corner bean part and let's have a look at it more closely. Click on the pot and press open part. And then when we're in the part, Let's edit that first sketch, the beams sketch. Now the problem is when we first made this part, ours a little bit lazy, I didn't measure everything. I assume that because the distance between these holes along the bottom is eight, then it will be the same egg millimeters between these holes going up the diagonal here. But if we think about this logically, because of the angle that won't work properly. We want the distance between two sets of rows to be a multiple of eight. And we also want the distance between two sets of columns to be a multiple of eight. If I add in some dimensions, we can see that we're off, they're saying 16.9 when it should be 16 exactly. This diagonal corner section must be to lower. And actually, if I go back to my Lego part and I measure it properly with the calipers is smaller than eight millimeters. I can now delete that dimension and I can fix it. We should have 16 between these two holes. And then because we've got a 45-degree angle there, it should also be 16 between these two sets of holes. And now if we measure this, we can see that's actually a little bit less. We had that down as eight is actually more like 6.6. That's where our problem lies. Let's make that change and then exit the sketch. And this is the beauty of SolidWorks. He can go back to any stage in your model and you can make changes. And then that can drag through to your final finished assembly. You don't have to start everything again from scratch. Now let's go back to our assembly and see how that affects things. Your assembly should update automatically. If it doesn't, you can rebuild by pressing Control B or pressing rebuild up hand. So if we zoom in a bit, we can see we've No Logo got clash on the gear that we had before. And also it looks like the axial and the axial whole are lined up left, right as we're looking at it. But there's still a bit off up, down. So we're getting closer to the correct solution, but we've still got a bit of a problem. So let's get the measure tool and we'll see where we are still going wrong. Let's say measure between these two axons here. So the distance here should be 8 to fit in with that standard eight millimeter spacing. But it's actually coming out as 7.6. And the reason is this axle with a ballpark is actually sing too far down in that ten sub assembly that we made in the last video. Let's open that sub-assembly and fix this. I'm just gonna click on one of the parts are can see where the sub assembly is in the parse tree. And then I'm going to click on stage ten and press Open sub-assembly back in our sub-assembly. So the vertical distance between this circle and this circle should be eight millimeters. If we get the measure tool, we can see that 7.6, we need to move that section up zero-point for. To do this, I'm gonna expand the Mate. I'm going to delete that coincident mate that we've already added. You could also just edit it and change it to a distance mate. If you hover over them makes their surfaces should be highlighted, so you should be able to find the correct one. Now if we try to select the two circular faces and make those a certain distance apart, eight millimeters. Then you find that we can't really do this because the distance mate is trying to set the shortest distance between them, which will be a diagonal line. We actually just want a vertical line. If we can't animate directly, instead we can use the planes. Let's find the plane that goes down the middle of the axle with ballpark. And also find the plane that goes down the middle of the cross block three long part. And then we can just add a distance mate that is eight millimeters there. We do have a small gap in-between those two parts now, but we know that the actuals are at the correct spacing. Now let's save that sub-assembly. Let's use Control tab to get back to the main assembly and see how we're looking. Right? We can now see from the side that the axons are lined up correctly. However, we've still got one final issue. This axial part with a sensible seems like it's slightly too wide because it's making these two beam with axial part clash with that latest for being with the extension part that we added. Let's open the axle with ballpark and have a closer look at it. Now if I double-click on that middle feature, we can see the width of it is 9.6. And actually it's another case of me being lazy. I didn't measure this properly. It should actually be smaller for this one, it should only be 7.4, which is that standard width of the block. You should be able to double-click on that 9.6 and then change it to 7.4. If you can't do it directly there in the graphics area, you can also edit that middle feature and just change the width of the mid-plane to 7.4, then the diameter of the actual circle should also be a bit bigger. So if you double-click on that, it should be 7.4 as well, not 5.9. It should look more like this. Now let's save that part and go back to the main assembly and see how it looks. Yes, now we can see everything lines up correctly. We do have a small gap in there. That's okay. That's just for the tolerance between the parts, maybe where they're being measured slightly differently to each other, or maybe just to allow them to fit together properly without being too tight. This stage is now done. I just wanted to show some examples of even when you're making parts that you think you know that I mentioned off, always be careful and maybe double-check your dimensions as you go. In the next section, we'll go onto stage 12, which only involves two new parts. And they're both pretty simple. 35. Creating the 7-Long Axle Part: We're now onto the second sheet with the instructions. And we wanted to stage 12. For this one, we only need to make two new parts. And the simplest one is just an axial that seven long. Let's open the existing axial part and add a new configuration on the Configuration Manager tab. We've already got 369. We now need to add seven. Right-click on the actual filename there at the top, and then press Add configuration and cool this new 17 long. Now make sure your seven long configuration is active. You can double-click on the name if it's not, and then go back to the design tree. Then click on that first feature, the extrude and press Edit Feature. Now down here and make sure you're on this configuration. You should be on that automatically. And then we just need to change the length. It should be 55.5 millimeters. Then you can just press Okay. Now we've added that extra length and we can go back to the Configuration Manager. We can just change the color. Make sure you're on the seven long configuration. Go to the Appearance scenes in details tab. And let's just make it a yellow. Now we should have 3679 and then you can just save your part. So that's all there is to that one. Probably one of the simplest ones that we've done. In the next video, we will be creating an axial joint that lets you join two axons together at 90 degrees. 36. Making the Axle Joint Part: We're now carrying on with Stage 12. And for this one we're making the axial joint part. This is a little bit harder than the act, so we just made, but luckily we've got a part of this halfway there. That's the large bush part. Let's open that from within the assembly somewhere. And then we'll save that and make some changes. Go to File Save As, and choose save as copy and open. And I'm going to put the filename down as axial joints. We need to now add another section to this part that can hold an axial perpendicular to the first one. To start off, let's start a sketch on the front plane. Let's get the circle tool and draw a circle about here. That should be 5.7 millimeters diameter. It should be lined up vertically with the origin. And then the distance to the center of that circle from the bottom of the existing power is 11.9. We can then do a mid-plane extrude 7.8 millimeters. And I'm going to call that middle top. Next we're going to add the rims. I'm gonna start a sketch on either of these n phases. I'm going to get the so-called tool, and I'm going to draw a circle that's a little bit bigger. This one should be 7.4. Then we can do blind extrude Warren 0.4 millimeters and make sure it's going inwards like this. This just adds that rim on the end. So I'm gonna call this one top rim. We can then mirror this over because there's one on each side. So let's select that top Room feature. Let's select the plane down the middle. So for me this is the front plane with both those items selected. Press mirror, then press Okay, if the preview looks good. Next up we're going to add this section that joins these two bodies together. Start sketch on this plane, the right plane. Then go Normal To and get the line tool and draw a sketch something like this. Start or the midpoint here. Go out to the left horizontally, a little bit beyond the end of that existing body. Then go downwards and pick up the outer line of the second body to about here. Then go over to the right horizontally to pick up this edge. Then go vertically up to this end, then get back to the midpoint, and then go back up to the start point. Then this line on the left-hand side should be exactly vertical. So you can click on that and out of vertical relation, this should give you a sketch which is almost fully defined. We just need to add one dimension. Let's just get smart dimension and adding one millimeter here. You should have a closed profile, something like this. We can then select this align in the middle. Then here on the left, choose for construction. That turns this solid line into a construction line. We can then select everything in the sketch and we can press Mirror Entities, and that will mirror everything we've selected about that center line. That should give you a solid profile that looks like this. We can then extrude this shape using a mid-plane extrude. So let's go to Features extruded boss base. Let's give mid-plane and 5.7 millimeters is the same as the inner diameter at the bottom. I'm going to call that feature something like axial joint. Next, we just need to cut away this curved section here. I'm going to start a sketch on this flat face. I'm going to go normal too. And I'm just going to get a corner rectangle. I'm going to start from this corner and go down to this corner. And that should fully define your rectangle because the opposite corners are fixed. We can then just go to Features extruded cut, and let's do a blind cut in this direction away from the main body. It doesn't really matter what the distances as long as it cuts through that curved section, I'm just going to leave mine as about five there. We've now cut away the extra section and the joint is exactly the same size as that lower diameter. I'm going to call that one side cut. And we then want to mirror this over to the other side. Select the side cut, select the plane that goes down the middle of the model. This should be the right plane. And then press mirror. And if the preview looks good, press okay, so we've now cut that curved section on both sides. Next up there's a little wall inside this gap here. To draw this, start a sketch on the right plane and then get a corner rectangle. And let's just draw from the bottom corner here up to this corner here. And again, not should fully define your rectangle because you've defined the two outer opposite corners. Then let's do a mid-plane, extrude 1.4 millimeters mid-plane and press Okay. And let's call that something like middle wall. Now the bottom of this overhanging phase is actually angled. Probably don't really need that extra detail, but we're going to add it for completeness anyway. First I'm going to select the plane that goes down the middle. This should be the front plane. And with that selected, choose the draft feature from the Features tab. This feature lets us how to draft angle to a face. We should have the front plane selected here. And then for the faces to draft, let's just choose this face here. And we'll set a draft angle of 30 degrees and press Okay. And it should add, if we look from the side, a slight angle like this. If you find that your angles in the opposite direction, what you can do is edit that draft feature and then just flip the direction. You can do that just by pressing this reverse direction box. Then let's just add the same on the other side. So let's select that plane again, the front plane. Also select the draft feature and then choose the face you want to draft and set three degrees. And you'll have to reverse the direction on this side compared to the other side because we are drafting in the opposite direction. If we look from the side, it should look something like this with those two angled edges. Next step, we can actually cut the actual hole. Let's start a sketch on the front plane. Let's go Normal To and draw the axial cut that we've drawn loads of times. Now, he starts with a circle that's 4.8 diameter. And then there's two sensor rectangles that are the same width, That's 1.8, then the length of them is set by making them tangent to that circle. We can then do an extruded cut and we can go through all both. And we can select in the selected contours, all five of those areas of the cross to cut out. When you've made that you can call it axial cuts were now almost done. All that remains is to add the slot through the middle of the top. Start a sketch on the right plane and get this lock tool and get a center point straight slot, and draw it roughly in this position. For the size, it should be one millimeter high. It should be 3.8 long along the middle of the slot. The middle of the slot. So the center point is lined up vertically with the origin. And then the position to the middle of this law is 11.9 from the very bottom of the pot. Then to finish off, we can just do an extruded cut through all both. And let's call that one top slots. This part is now complete so you can save your part. And in the next video, we'll use these parts to complete stage 12. 37. Stage 12: Adding the Main Rotor Shaft: Now that we've made those two new parts, we can start to make stage 12. As usual, we start with the small substage. Make sure you've got the parts that you need open. We should have the axial, the large bush and the actual joint. I'm going to go to the axial and I'm gonna go to File make assembly from parts. I'm going to pin the insert components menu open, and then I'm going to insert the axial first. So that's fixed to the origin. It doesn't matter that it's the wrong size. We'll fix that in a moment. But first we'll insert the rest of the parts. I'm also going to insert one more Axel. I'm going to spin that around to the correct orientation. And then the actual joint that should be in this kind of orientation. Again, it doesn't matter if you don't get these exactly right because you can rotate them around when you're adding the mates. Then finally, I'm going to insert that large bush as well. And I'm gonna spin it around like this. The end where the cuts should be facing downwards like this, which would be facing outwards from the screen. But again, you can spin that around later on if you need to. Now let's make these axons the correct length. Start with a fixed one, will make that seven long. Click on the part and then from the drop-down, choose the seven long configuration. It should be the one that's yellow in color. And then for this one at the top, we can click on it and that should be three lung. Then we can just make our parts together as usual. Let us select a circular face on the actual joint and then a similar circular face on the axial. Let's make those concentric and lock the rotation. If you find that your parts aren't lined up properly, you might need to select a flat face on the axle and a flat face on the joint and then make those parallel. Then for the position of the actual joint, I'm just going to drag it out so we can see inside it. Then I'm going to select this inside face at the top. And then also select this top face of the axial. And I'm gonna make those coincidence just so that it's touching. Next, I'm going to make this large bush concentric with the actual joint. I'm going to lock the rotation again. Then I'm just going to drag it down and I'm going to make those two faces coincident so that they're touching. As I mentioned, the end where the cuts should be facing down to the open-ended the axial. It doesn't really matter too much if you get it the other way round, but that's just what the instructions say. And then finally, let's select that small axial and let's make that concentric with the actual joint. We can lock the rotation and then we can move it to the middle. We can meet it in place using the plane that goes down the middle of the actual, also the one down the middle of the assembly. We should have something like this. We've got the large axial, then on top of it we've got the actual joint with a small axial going through it. And then underneath that we've got that large bushing just as a spacer. We can then save this silver assembly. This one should be called stage 12. We can now go back to the main assembly and insert this sub-assembly. Let's use Control and tap. Then let's go to insert components, will find that latest stage 12 and insert that subassembly. The axial goes through this hole here, rotate your model around and select that whole. And then also choose a circular face on the axle and make those concentric. Now we don't need to lock the rotation for these because we actually want this axle to spin around and this is how the helicopter blades rotate. Then let's just set the height. So let's choose this top face and then the corresponding face on the bottom of the bush. And let's make those coincidence so they're touching each other. So you should see that this new stage 12 assembly can spin around within that hole. Now if we look at the instructions, There's also another gear that goes in this gap here. In real life, we have to insert this as we slide the axle through. But in SolidWorks we can just start it afterwards. To add the extra gear, Let's copy one of the existing ones. So hold down Control, left-click and drag from an existing gear and then release to add that new part. First, I'm just going to rotate it to about the right orientation. You can do this by holding down the right mouse button and dragging the part around. Then let's select one of these circular inside faces and a corresponding one on the axial, and let's make those concentric. Now we do want to lock the rotation, but you probably find that your axial and you gear aren't quite lined up like this. So to fix this, let's just choose a flat face inside the gear and then also a corresponding flat face on the axle. And let's make those parallel. We can then just move this gear up to the correct position. Let's put it in the middle here somewhere. Let's just select this upper face of the gear and the lower face of the beam here. And let's make those coincidence. This stage, these two gears aren't meshed together properly, so they don't actually affect each other. But that's something we'll fix once we made the whole assembly. But for now you can save your assembly and stage 12 is complete. 38. Stages 13, 14 and 15: Building Up the Other Side of the Helicopter: We're now onto stage 13, but we're actually going to do 131415 in one single video because they're all fairly simple stages. And we've made all of the parts that we need already. If we look at 13 first, this little symbol on the instructions means we have to spin the model over. Let's rotate our SolidWorks model. So we're looking from the underneath like this. We now need to add one more gear and one more large bush. First, let's find the large bush. There's one in the middle there. Let's hold down control and left-click and drag from that Bush and then release and that she would insert a new Bush part. Then let's find a gear and do the same thing. Hold down Control, left-click and drag from the PAR and then released to add that new part. We can then make those in place. I'm going to start with the large brush. I'm gonna rotate it about the correct orientation by holding down the right mouse button and dragging the part around. The curves should be facing downwards. Again, it doesn't really matter too much if they're not. But that's just what the instructions say. Then let's select a circular face on the bush and also on the axle and make those concentric. We do want to lock the rotation, but if you're a bit misaligned like this, you might have to zoom in and select a flat face on both the bush and the actual and make those parallel. Then let's just choose this top face of the Bush and then the bottom face in the beam and make those coincident so that they're touching. Then let's do the same for the gesso, rotate it around, choose a circular face inside the gear and also circular face on the axle and make those concentric. Then choose a flat face on the axle and a corresponding flat face inside the gear and make those parallel. Then let's just make the bush and the gear coincident. It should be something like this. This gear is just on the bottom to give you something to grab onto so you can actually rotate the blades with your hand. That stage 13 complete. Now let us look at the instructions for the next stage, number 14. For this one, it says we want to spin around again. So we're going to rotate the model again back to the original view from the top. And if we look at the picture, what we're going to do is add on another of those white corner beams. And then we're going to add on to small bushes. But we've already added them on one side, so perhaps we can just mirror them to the second side. First, Let's select the mirror feature. So go to Assembly, click on the drop-down underneath linear component pattern and choose mirror components. The mirror plane we want the plane that goes down the middle of the assembly. If you expand this second feature tree here, we want this one which is the right plane. Then for the components to mirror, we want to zoom in. We want to select these two small bushes. We also want to select this white corner beam. But if we click on that white beam, you'll find that we actually insert the entire stage, all of stage one. And we only actually want to mirror one single part. The problem is because that part is within a sub-assembly, we can't just mirror that specific part. Instead, what we'll do is just close the mirror and then we'll just insert a new white part, not as a mirror, just as another part. And then we can mirror over the bushes after that. To add that new white corner piece. Let's hold down control and left-click and drag from the existing one and then release and that will insert a new part. We can then make this in place properly using the existing holes. Let's select inside this first hole on the beam. And then let's also select a circular face on that front axle. We will align those up concentrically and we're locked the rotation so that part can't rotate. That should put us in the correct place. And then we just need to set the left-right position. We actually want the outside face of that green pin to be lined up with the outside face of that white beam. So let's move the beam in a little bit. And then let's choose these two faces and make those coincidence. So we've now added that second side of the body there. Now we can use the mirror to add those two small bushes. We can do this because these are just individual parts within the main assembly than not sober assemblies. You can mirror subassemblies, but you can't mirror specific parts from sub-assemblies to mirror these small bushes. Let's select the plane that goes down the middle of the right plane. Hold down Control. And let's also select those two small bushes. Then go to linear component pattern and choose mirror components. Here we've got the right plane, we've got the two small bushes. Let's click Next. That preview looks good. So let's press. Okay. Now we've added those two small bushes and we completed stage 14. Moving on to stage 15, This is pretty similar. We just need to add two new parts from one side to the second side. These are the four beam with extension, which is an individual part, and also the right angle beam width curve, which is also a car. So we can mirror both of these over. And instead of creating a new mirror, we can just add these to the existing mirror that we made in the last stage. To do this, go down to the bottom of the parts tree and click on the mirror feature and press Edit Feature. Then make sure you're in this components the mirror box, and we can just choose the extra parts that we want to mirror. Let's choose this first one, the right angle beam with curve. And then also choose that one at the back. That's the full beam with extension, we should now have four items in this components to mirror, to small bushes, the right angle beam with curve and the full beam with the extension. Then you can press Next. And the preview should look something like this. If you find that one of your parts looks a bit back to front, like it's the wrong way round. What you can do is find the part here on the left and then choose the correct orientation from these options underneath. Now if you're on an older version of SolidWorks, your interface might be slightly different here, but there should be different options for you to choose the orientation of the power. There should be three orientations that look completely wrong, like the part is back to front. And then there should be one of them where the part is the correct way round. So just choose the correct option and then press OK. And those parts are mirrored and we're really building up the shape of the chopper. Now, if you find that when you have made the mirror, one of your part's easy in the wrong orientation. You can just go down to the bottom of the part street and edit the mirror feature and then change the orientation within that mirror feature. You can then save your assembly there. And in the next video, we'll go onto stage 16. 39. Making the 2-Long Axle Part: We're now on stage 16. And for this we need to new parts. The first one is pretty simple. It's just a smaller axon with some extra details. The second one is probably the most complex part we're going to make, but we'll start off with an easy one, the axon, let's open an existing axons can be any size, and let's make some changes to that. We need to add a two long configuration. Go to the Configuration Manager and right-click on the part name at the top and press Add configuration for the new part name. Let's call it too long with cars because there are some extra details come out of this smaller axon. Make sure you've got that two configuration active and then go back to the design tree. First of all, set the length. So let's edit this first feature. Make sure you're on the disk configuration option down here should be on that automatically. Then set the length as 15.6 millimeters and press Okay. So at this stage it's pretty similar to the other axis, is just shorter. If we look at the part though, it actually has small cutouts that go round as well. To make these will do a set on one side and then will mirror it to the other side. Let's start sketch on the plane down the middle for me, it's the front plane. I'm going to go normal to get the circle tool and just draw a circle at the origin. This should be 3.8 millimeters in diameter. We'll now use this circle to cut away the extra material that we don't need. To do this, let's go to Features extruded cut. So we want to cut blind one millimeter deep. We want to select this option flip side to cut. So we're gonna cut everything outside of the circle. So it's gonna be these extra areas out here. We also want to offset where the cut-offs, it shouldn't be in the middle. To do this, let's go to the left and clicking this from drop-down and choose offset. The offset length can be 3.5 millimeters. You can go in either direction. It doesn't really matter, but we want to be cutting outwards. You might need to flip the direction of your car. If we look from the side of the curve, should be going outwards to the end of the axon. This coding line, this arrow here should be pointing outwards like this, and not inwards like this. Then let's press Okay to make that cut. And you should have these four ridges cut out like this. So it doesn't go all the way down. It's just a little extra cup. And I'm gonna call that feature side cut. We then just need to add this to the other side as well. I'm going to select the plane that goes down the middle of the front plane. Also select that side cut and press mirror. And then the preview looks good. So I'm going to press Okay to add that to the other side. Now if we go back to the configurations and we go through them, we should see that sidekick hasn't affected any of the other configurations. This is because we made that feature in the two long configuration, the features that you add will only be added. So the configuration that you are active in, unless you turn them on later in the other configurations. Let's go back to that too long with cuts that we just made. And let's just change the color. Go to the Appearance scenes in details tab, and let's make it a red. Now we should currently have the two, the three, the six, or 79. You can then save this part. In the next video, we'll go on to that tail rotor part, which is fairly tricky, but we'll build it up stage by stage. 40. Creating the Tail Fairing Part: The next part that we're going to make for Stage 16 is a bit of a non-standard part and it's probably the most complex one we're gonna make in the entire course. The tail fairing that fits on the end of the helicopters tail. Let's start a new part and get started with this star sketch on the top plane. And we'll start off drawing a section that has the two blocks because we know they're a pretty standard size. Let's get the slot tool uses center point slot and draw a slot at the origin like this. It should be 7.4 high and then 15.4 across the entire length. Remember if you hold down shift, you can dimension to the outsides of the slot, then I'm just gonna do a blind extrude seven millimeters. This doesn't have to be mid-plane and I'm gonna go downwards like this. And let's call that feature to block body. Next, I'm going to make an entirely new body for the area where the actual fitting. Start a sketch on this plane that goes down the middle, the right plane, then go Normal To. And let's draw something like this. Start off with the circle tool. Draw a circle that's lined up with the middle of the part like this. And then we'll get the line tool and we'll draw three lines coming off it on the bottom like this. The center of this circle should be vertically aligned with the origin. It should be touching the top edge of this part. So let's select the circle and that top edge and make those tangent. The diameter should be 7.4 in size. It's the same as that first body that we made. And then to this bottom line from the very top of the part should be 10.2 millimeters. We can then extrude this, but we need to offset where the extruded. So let's go to extruded boss base. Firstly, in the selected contours, we need to choose both of those areas. It's the rectangular area at the bottom, and it's also the circle at the top. We also need to offset the start point here on the left. Let's go to from, let's choose Offset. For the offset distance will make this 24 millimeters. It will then do a blind extrude, and this is 7.85 millimeters. The direction of it should be going back towards the existing body. To check the size. Once we made that new body, we can get the measure tool and the entire length here should be 31.7. I'm going to call that feature acts or body. Next we're going to draw a sketch on this end phase to cut the axial L. But we're not actually going to cut the actual yet. We're just gonna use that sketch to line up some other features. First, let's start sketch on this N face and let's draw that usual actual profile that we always draw. We've got a 4.8 millimeter circle in the middle. Then we've got our two center rectangles will make those the same width, which is 1.8. And then we'll link those to the size of the 4.8 circle by using those two tangent relations, we also need to cut out some more material for the cavity. To do this, we're gonna select that small circle, the 4.8. And let's offset that outwards 1.3. That should be touching the outer curve of that new body that we made. Then let's get the circle tool again. We'll draw another circle down here directly below the first one. We'll make it the same size as that large one. So you can select both of them and make them equal. It should be lined up with the origin vertically. And then the distance between the two circles should be eight millimeters. That should fully define that circle will also offset these outer edges inwards one millimeter each. Do the right-hand side and also one millimeter on the left. Then it's also get the line tool. And let's just extend these lines downwards. This just gives us the full profile of the area we need to cut out for the axial and the cavity. We are going to count this cavity, but before we do that, we're going to make the fairing. So let's exit the sketch, then start a sketch on the same end face. Firstly, I'm going to select this outer top circle and press Convert. So we've now got that in our new sketch. Then get a center line tool and just draw a center line down from the very top of that circle down to the center point and then directly out to the left. We can then use the trim tool. Make sure you're on power trim, and we can trim away the rest of that circle. So we just want that top left quadrant. Now the reason we drew the other axial cut sketch first is because we're going to use the lines within it to lay out this other sketch that we're in now, make sure you can see the actual sketch. You should be able to see it by default. But if you can't, you can click on the Sketch and press Show. Then hover over the sketch, and let's choose this left-hand vertical line, then press Convert, and that line is now added to our current sketch. You can then select the line and on the left here press for construction. We'll also select that lower circle and convert that. And then also make that for construction. So click on it and then choose for construction on the left. Now we know that the fairing kind of curves inwards. We also know that the thinnest part of the wall is 0.6 at the very bottom. I'm going to select that vertical construction line. I'm going to offset 0.6. I'm gonna make the offset line into a construction line as well. And then press Okay, I'm also going to get another center line and I'm going to draw a line out from this intersection of the inner line and the circle directly to the left, we should have something like this. We're going to use this point on the left as a guide for the curve of the fairing. And this will all become a little bit more clear in a moment. Let's get the Arc tool. Let's choose a three-point arc. And let's start an arc from the bottom of this existing arc at the top and go down to about here. And then pull out and set the arc, something like this. Then select that top arc and the new arc that we just drew and make those tangent, those two arcs now join each other with the same curve. Next we'll select this end of the small line. Will also select that new arc that we drew and we'll make these coincident. That means that the arc now goes through that point that we selected. And then the total height of this part we know from measuring is 15.4. I'm going to get the smart dimension. I'm going to add a dimension from the very top of the part to the end of that long arc on the bottom, you should have something like this. Both of those arcs should now be fully defined. This gives us the outer curve of the fairing that we're going to extrude. To set the wall thickness of it. Let's select both of those arcs. And then let's offset Warren 0.5 inwards. Make sure that the offset line is solid and also the baseline is summit. You should have something like this. And then just get the line tool and let's just close the profile. So let's draw a line across here and a line across here. Let's also draw another line along here where the two arcs join. Because we're actually going to extrude two sections of this profile separately. So you should have a fully closed profile like this with a line across the middle as well, which breaks it into two profiles. Now from within the sketch, let's go to Features extruded boss base, and let's just extrude that top part of the profile. So let's choose that top part and the selected contours will flip the direction. So we're going back towards the original body. From the end conditions, Let's choose up to body. And then let's choose that first body that we made. Your preview should look like this. You can call that feature fairing top. We're now going to extrude that bottom section of the profile, but we're going to extrude this one a little bit further. Expand that fairing top feature and underneath that you should see your sketch. We can reuse this sketch again in the next feature. Select that sketch and then choose extruded boss base. Then in the selected contours, Let's choose that bottom part of the profile. You might need to click into two areas separately. Then let's flip the direction and we'll just do a blind extrude 38.2 millimeters and press. Okay. It should look like this and I'm going to call that feature fairing bottom. Next, we can cut away these little areas that are sticking out. So let's start a sketch on the front plane. Let's go normal to select this lower arc curve and press Convert. Then just drag that top end of the lineup so it joins exactly with the outside of the part. Should be just where this top curve start around there. Then get the line tool and just close that profile with two straight lines, one horizontal and then one going vertically up to that top point. We can then use that profile to cut away. So let's go extruded cut, let's go through all both. And let's call that fairing side cut. Next, we can fill in this top part here. So let's spin around. Let's start a sketch on this face. Go Normal To get the rectangle tool and a corner rectangle. Let's start from this bottom corner and go up to this top edge like this. And then you can drag this bottom left corner to the corresponding corner on the existing part that should fully define your rectangle like this. Then let's just go extruded boss base. Let's flip the direction so it's back towards the rest of the part. We can choose up to next. It should look like this. Press, Okay? And let's call that fairing corner. Next, we can actually cut away the axial area. Let's go and get that original sketch that we drew, Sketch three for me. Let's do an extruded cut for the selected contours. Let's zoom in and choose those five areas of the axial cut. Will also choose the rectangle part at the bottom and the two small wedges. And then we'll also choose that currency area, which is sort of like a wedge on its side. Then for the end condition, Let's choose up to surface and will choose this surface here. Now the reason we didn't make this cut before we made the fairing is because the fairing would have actually filled in some of that car. Let's call that something like axial cuts. Next we can round off the edges inside the actual curves. So let's get the fillet tool is 0.5 millimeter. Fill it and let's round off these four inside edges. Next we can cut the holes on the original block. So let's start sketch on this top face. Let's add two circles, each one concentric with the outer curve of this law should be the same size and they should be 4.8 millimeters. Again, we didn't cut these first because when we added the fairing, it would have filled in some of those holes. Just as a double-check the distance between them. It should be that standard eight millimeters. Then we can go extruded cut, and we can just choose up to surface. And we can choose this bottom surface here. So it's just cutting through the original block. Let's call that one block holes. Next there's a wider rim on the top of these holes. So let's start another sketch on the same face. Let's select those two edges and offset them. And if you find that you can't offset them, you can convert them first and then select the converted lines and offset those. The offset distance is 0.7 outwards. We can then use those larger circles to cut that rim. So let's go extruded cut, Let's just go blind 0.5 millimeters. We can call those rim cuts. We've built up a lot of the shape now there's a bit more to do them. We've got one more detail on the backside here. This is a small stopper underneath those holes. Let's start a sketch on the front plane. Get a center rectangle, and draw a center rectangle about here. The size of this is 13 millimeters long. It's 0.50.5 below the bottom of that first block that we made. And then the center of it should be lined up with the origin like this. It should be that kind of position and should be fully defined. We can then go to Features extruded boss base. We actually want to extrude it from that curved surface. Here on the left. Let's go to from the drop-down, let's choose Surface, face or plane. And then we can choose that surface there. Then let's just do a blind extrude upwards 0.5 millimeters. You can call that stopper. We're nearly there now. Just a few more details. Let's get the fillet tool. Let's add a one millimeter fillet on this end here. Now we can cut that fairing curve to the exact shape from the side. Let's start a sketch on the front plane. Go to a normal to view like this. We want to be looking from this side, from the back. You might have to press normal to twice to flip your view around. Then get aligned tool and draw something like this. Start from this top right corner, go out to the left horizontally and then go down and join the outside edge and then go vertically up to that corner again. The top-left corner of this triangle is 3.8 from the original body, and the height of the triangle is also 3.8. Then get the line tool again and draw a vertical line going down from the bottom of that triangle that we drew all the way down to the bottom corner of the par. Then horizontally over to the left, not quite to the far edge, but just to the edge of this fillet like this. We can then zoom out a bit. We can go over to the right, put a point here, and then go back up to the start point with another line. Then for the dimensions, this point here is 2.5 from the edge of that original body. And then the distance from the very top is 10.4. That should fully define your sketch. Will then cut away these two enclosed sections. So let's go to Features extruded cut in the selected contours. Let's choose this top triangle, and we'll also choose this bottom profile. We can do through all both. And that should give you that fairing shaped like this. So we can call that fairing main cut. Now let's just add a few fill it. So get the fillet tool. Let's add a five millimeter fillet on this bottom edge. And this is a little bit of an approximation, but it's good enough for our purposes. Then let's get a one millimeter fill. It will add it onto this sharp edge here. And then I'll say these three edges on the right-hand side here. Then the modelling is finished so you can save your part and let's call it something like tail fairing, 30465. Then finally, I'm just gonna change the color. So let's open appearance scenes and details will choose a medium gloss plastic. We'll make it the green color. And then we'll go in, we'll edit that grain to be more like that lime green of the original pause. Then this part is totally finished, quite a long video there, but the next one is much simpler. 41. Stages 16 and 17: Making the Tail Section: In this video, we're going to create Stage 1617. They're both fairly simple stages and follow on directly from each other. Make sure you have all of the parts that you need open. So we have the tail fairing, the friction pen, the axial and the cross block three loan to start off, I'm going to go to the axial part and I'm going to go to File make assembly from part. Then as usual, I'm going to pin the insert components menu open. And I'm gonna insert all of the components. I'm gonna start off with the axial. It doesn't really matter that this is the wrong size because we can change that in a moment. Then I'm also going to insert the tail fairing. Spin around. Next is the cross block three long. I'm going to spin that around as well. And at this stage I'm also going to insert the friction pens. And there's two of those. We can then close the insert components menu and start to put everything in the right place for the axle. I'm going to click on that and I'm going to choose that small configuration that we added that to long configuration. Then I'm going to make the axial concentric with the actual toll on the fairing. Sort of hard to see exactly how far this axle goes into the part. But what I'm gonna do is expand the axial part. I'm going to choose the plane that goes down the middle. So that's the front plane. And then I'm just going to make that coincident with this outer face of the fairing. I'm also going to lock the rotation of the axle. So I'm going to expand the Mates here at the bottom. I'm going to right-click on that first concentric mate, and I'm going to press lock rotation. Then I'm going to make that cross block in place using similar principles. So I'm gonna select a circular face, also a circular face inside the actual hole. I'm going to lock the rotation. And then I'm just going to make these two faces coincidence. It should be something like that. And that stage 16 done. Then for stage 17, we just need to add these two friction pins. I'm going to choose these two faces and make those concentric. I'm going to lock the rotation and then I'm going to drag the pin down. It's a little hard to see how far these one should go down. They actually do stick out with the bottom a little bit. So it should be something sort of like this. What I'm gonna do is go up to the top of the pin. And then I'm going to choose this bottom face of the rim. Then I'm also going to choose this top face of the inner wrinkle on the fairing. And I'm going to make those coincident. Then it's exactly the same for the second pin. So first I'm going to make it concentric. I'm going to lock the rotation. And then I'm going to choose that interface and then the bottom face of the rim. And I'm going to make those coincidence. So it should be something like this. Then we can save this assembly as stage 17. In the next section, we'll go onto stage 18 and we've got to make three new parts for that. 42. Making the Pin with Axle Part: Welcome to stage 18. For this, we've got to make three new parts. And the first one is pretty simple. It's just the friction pen has got an axial that's two blocks long on one side of it. First I'm going to open one of our existing friction pins. I'm going to spin around and have a look, and there's one underneath here. So I'm going to click on that and press open part. Then let's save this part as a copy. So go to File Save As, choose save as copy and open. And I'm going to call it friction pen with long axial. We can then close the original document and now let us make some changes to this new part. Firstly, I'm going to drag up to that middle ring, the first feature. We actually only want this to be half the thickness it is now. We only want it to go in one direction instead of mid-plane. Let's edit that feature. Let's change it from 1.6 down to 0.8. And let's change it from mid-plane to blind. Then you can exit that feature and we can go down below the next one, the outer body. This one also needs to be half the thickness and also just going in one direction. So let's edit the feature for the value here. We can divide this by two. So just click in the box and after the number, just put slash two and then press Enter. That will divide that number by two. So that should be 7.35. We can then make this blind instead of mid-plane for the outer rim. Let's keep that the same. Then for the mirror feature, we no longer need that because we've just got the rim on one side so we can delete that. The middle slot, we don't need that either. You can also delete that and you can delete the sketch underneath that. Then for this slide slot, we can keep that as it. We've got the pin half of the part. Now we need to add the axle to the other side. To do this, Let's start a sketch on this face and we'll draw our usual axial shape. Get the circle tool, draw a circle at the origin, that's 4.8, and then draw our two center rectangle's. Hopefully not too bored of this profile yet. They should be 1.8 wide. And then the length of them is set by adding those tangent relations to link them to that full 0.8 circle. Then when you've got that profile, we can extrude it as normal. So let's go to Features extruded boss base, and in the selected contours, Let's choose those five areas of the cross. You might also need to click on these outer areas as well, just because of the way the sketch is made. We should have something like this. Now the total length of this part is 23.8, but that includes the area of the pin that we've already made on the left. We don't actually have to calculate the length that we need to extrude this side. Instead, we can just use offset from surface to do this, go to the end condition drop-down and choose Offset from surface than in the surface box. Let's choose this end phase here. Then for the offset distance, we can write in 23.8 millimeters. Then you might need to flip the direction of the extrude by clicking this reverse direction box here. And you should see a preview, something like this. Now if you can't see this, you might need to press this reverse offset box here. If you can't see preview dry unchecking that reverse offset box. This means that our Extrude is going a length of 23.8 millimeters from that face that we chose on the left-hand edge of the pen. Let's press Okay to make that as a double-check, you can go to the Evaluate tab. You can get the measure tool. The entire length here should be 23.8 millimeters. Then let's just call this feature actual. Next we can add those little fillet to the end of the axon. So get the Philip tool set 0.5 in size and just select those four outer edges, like we usually do for the axial part. Then finally, we've got a little gap here that we shouldn't have, so we're gonna fill that in. So just start a sketch on this face here. Let's choose the outer rim and press convert entities. And then let's just extrude that circular area 0.8 outwards in this direction. Just a fully fill in that base there, and let's call that axial base there. We have a friction pen on one side and a double axle on the other side. And we can save that. In the next video, we'll make the tail rotor. 43. Creating the Tail Rotor Part: The next part that we're going to make is the tail rotor. This looks like it could be a fairly complicated apart, but it's actually alright, once we get into it, Let's start a new part and start sketch on the top plane. And first let's draw that in a REM. We can do this by drawing two concentric circles. The inner one is 4.8 millimeters and the outer one is 7.4. Then do a mid-plane extrude. And the width of this is 7.8 millimeters. And let's just call that feature hub. Before we start adding the blades, we're gonna cut away that top rim at the top of the hub. So I start sketch on this top face. Then select the inner circular edge and offset that outwards 0.7 millimeters. We can then do an extruded cut, so we'll go downwards 0.8 millimeters. And let's call that feature rim cut. Now we have this on both sides of the hub. So let's select that rim cut feature. Let's choose the top plane and then press mirror. And that preview looks good. So let's press Okay. We now have that feature on both sides of the hub. We can now actually start to draw the blade shape. Let's start another sketch on the top plane. Let's go to a normal two view. So we're looking directly down. Firstly, we'll add a center line because the blade is symmetrical. You can choose this from the drop-down next to the line tool. Let's start from the origin and just go directly vertically up. Then let's get the line tool and start to add our actual blade shape. I'm going to draw profile something like this. Let's start at this point where the center line goes through the outer rim, go directly out to the side horizontally, and then go up and left. And then go up and write like this. And then go back in horizontally to the middle to where the center liners. We can now mirror this off with a sketch to the other side. If you press control a that will select everything in the sketch. Because we've just got that one center line. We can just go to the Sketch tab and we can choose Mirror Entities and everything will be automatically mirrored around that center line. You should have this sort of enclosed profile that's kind of a coffin shape. We can now start to add some dimension. So let's get the smart dimension tool. The width of this first line along the bottom is four millimeters. This distance here is 2.85 millimeters. Then this widest width ear is 6.7 millimeters, and this width on the end is 5.25 millimeters. Then the total length here is 16.8, and that should fully define your sketch. Now actually if we look at the blade, the end of it is curved and it's a little bit longer than this. Let's select this small line here and make it for construction. You can do this by selecting the line and clicking for construction on the left. Then let's get the Arc tool and let's choose a three-point arc. And let's just go from the left-hand edge here over to the right-hand edge and just drag your arc out. So it's something like that. Let's set the height of this arc has worn millimeter. So you'll have to hold down Shift to dimension to the outside of that curve. We're now also just going to extend the bottom of the sketch a little bit. So we've got a root that goes into the hub. Let's click on this first line and make that full construction. Then let's go to the line tool and let's choose a midpoint line. You can get this by going to the drop-down underneath the line tool. This is a line that goes out equally in two directions from a midpoint. Let's zoom in. Let's start about here and go out directly to the side horizontally and make sure you don't get any of the automatic relations. So don't click on any of these curved edges of the arc. Then let's just get a normal line and we'll start at the bottom of this diagonal line. And we'll just follow the same angle down inwards like this until you hit that new line that we just drew. We can then drag it in the outer point of that midpoint line so that it touches that new diagonal line. Then let's just select that new diagonal line and also select the center line and press mirror. And then we should have that on both sides. So we should have a closed profile again. You should have something like this. If you find that your diagonal line is wonky, if it's not lined up with the diagonal line above it, then what you can do is select both of them and choose make co-linear. Then let's just fully defined the sketch by getting smart dimension and adding a dimension between here and here, and setting that as one millimeter. So we just want it a bit of extra material there to attach to the hub. And you should have a sketch that looks like this. We can now do a mid-plane extrude. Let's go to Features extruded boss base. Let's go to 0.2 in size and set it as mid-plane. But before you press okay, you don't want this new blade to be merged with the hub yet because we want to add an angle to it, you can make this into a separate body by unchecking merge result here on the left. Then if you press Okay, you can see here in the solid bodies folder, we've now got a two after it that indicates we've got two bodies in the model. And if we expand that folder, we can see we've got the hub and we've also got that new blade. So these bodies aren't connected to each other and we can make changes to them separately. At this stage, I'm also just going to rename that new feature as blade. Now if we look from the end of the blade, is actually got a curve to it on the top and the bottom. To add this, Let's start a sketch on the front plane. Let's go normal too, so that you can see the blade. You might need to press normal to twice so that you flip your model around. Now let's get the line tool and we'll start aligning this top corner on the left. And we'll go over to the top corner on the right. Then let's get the Arc tool and let's get a three-point arc will start also on the left-hand edge. And we'll go over to the right-hand edge and draw something like this. Then these two answer the straight line and the ARC should be lined up vertically. So select them both and press make vertical. And then the same on the right hand, they should be vertical as well. And then select the arc and select the straight line and make those tangent. So that just means that the arc exactly touches that straight line. Then the length here on the left should be 0.5. Now the ends here, they shouldn't be free to move in and out. They should be fixed to that widest part of the blade. Let's select one of those endpoints. And let's also select this widest edge here and make those coincident. And then let's do the same on the other side. Let's select this point and also that widest outer edge and make those coincident. If you were in a normal to view, then you might just be able to drag those to the correct line and add that automatically, but sometimes it can be tricky to add that. Then finally, let's select these two endpoints of the arc, and let's make those line-up horizontally. That should fully define your sketch like that. We'll then get the line tool and we'll close the profile by adding a small line here. And then the same small line on the other side. We also want to mirror this profile over to the bottom edge. So let's get a center line. Let's draw a line that goes out horizontally from the origin. And then let's just press Control a to select everything in the sketch. And then let's press Mirror Entities and that should mirror that profile onto the bottom side of the blade. We can now use this profile to cut away the curve of the blade. So let's go to Features extruded cut, the selected contours. Let's choose those four areas of the profile. There's two on the top and two on the bottom as well. For the end condition we want to use through all going in this direction. But before you press Okay, we actually only wants to cut through the blade body, not the rim body. Go down to the very bottom of the property manager here on the left where it says feature scope. Make sure you have selected bodies chosen and then uncheck that auto select box. If you don't see the feature scope there, it means that you've just got one single body in your model. You need to go back to when we extrude it that blade, and you need to edit the feature and uncheck that Merge Result box. But if you do see the features go, Let's uncheck auto select. And then let's just choose the body that we want to occur. So it's just the blade body. You can just click on that in the graphics area and you should see the blade body goes into the box down there. So this means a cut that we're making is only applying to that blade body. Press. Okay? And we can now see that we cut the curve on the top and the bottom of the blade. Let's call that blade curve. Now we want to give a bit of an angle to this blade. To do this, we can rotate it, but first we're going to add an access which will make it easier to rotate. We can add the axis using two planes. So first let's select the planes that we want. So for me it's the top plane and the right plane. Since the two planes that go through the middle of the blade with both of those planes selected, go to the Features tab, click on the drop-down underneath Reference Geometry and choose access. You should get a yellow preview like this for where the axis is gonna be added. If you don't see this, make sure you're on the two planes option here on the left. And just make sure you've got both of your plane selected there, the top plane and the right plane. Then if you press okay, the axis is added. We can now use this access to rotate the blade. And to do this, we're going to use the Move slash copy bodies command. You can find this in Insert Features, move slash copy. You can also search for commands using this search box up here on the right. To do this first click on the dropdown and make sure you're on the Commands option. And then just clicking the box and start to type in the name of the command you want. So I'm gonna start to type in move MOV. And we can see that the move slash copy bodies. We can now open this tool just by clicking on it up here. Now in the move slash copy body tool, if you're a property manager, looks different to this. If it looks like this, then just go down to the very bottom and click on this box that says translate slash rotate. So it should look something like this. First we want to select the body that we want to move. Let's click in this box at the top, and then let's select the blade body. We can then rotate his body around. Let's go down to the rotate menu. Let's click in the first box. This is the rotation reference, which is the point where you rotate your body around. Let's click on that box and let's choose the axis that we added. We now just need to set the angle of rotation around that axis. Let's try ten degrees so that blade looks like that, and that's not quite enough, so that's up to 15 degrees. And you should see a preview of the blade rotating slightly. Now make sure you don't have copy selected that would add a second body and then just press Okay. Now the blades at the correct angle and we just need to pattern it around so there's three of them. So let's go to the Features tab. Click on the drop-down underneath linear pattern and choose circular pattern. Before you do anything else, let's go down and let's click in this body is option because we want to pattern the entire blade body and then select that blade body to pattern. We want to set three instances. It should be equal spacing 360 degrees. Then we can choose the reference to pattern that body around, clicking this box at the top. And now we just need to choose a circular face in the hub. I'm going to select this inside face. And when you do this, be careful that you don't select the axis by mistake. You should see a preview like this. We're gonna pattern that blade around three times. Let's press Okay, and we've added those three new bodies there. Now if we look in the solid bodies folder, we've got four bodies. So we've got the hub in the middle, and then we've got the three rotor blades, which are all separate. We can now join these bodies into a single body using the combined feature. You can find this in insert features combine, and also you can use that search box on the top right if you want it. If I type in CEO and B, there's the combined tool. I'm going to click on that to select it. We're now in the combined tool for the operation type. Make sure you have add selected. This will just add all of the bodies together into a single body. And then for the bodies to combine, let's just choose all four of those bodies. It's the internal router and then it's the three blades. And then press Okay, and now we've just got one single body again. You can then save this part and I'm going to call mine tail rotor 30465. And let's change the color to that usual dark gray. In the next video will be making the half bevel gear that actually spins the tail rotor around. 44. Making the Half Bevel Gear Part: The next part that we're going to make is the half bevel gear. This is used to turn the tail rotor around, starting EPA and start sketch on the top plane. And first we're going to draw the main rim, get a circle and draw a circle at the origin. This should be 12.6 millimeters in diameter. And then we can just extrude this upwards, 0.4 millimeters blind. And let's call this first feature main rim. Let's start a new sketch on either side of this. Then get the circle tool again and draw two concentric circles. The smaller one is seven millimeters and the larger one is nine millimeters. And then let's just do a blind extrude with that ring shape. One millimeter. This is just a little ridge on the back of that gear. I'm going to call this rear rim. Then that spin around to the other side. Start a sketch on this face. Get the circle tool again and draw another circle. This one is 7.8 millimeters in diameter. Then it's a blind extrude 2.6 millimeters high. It should be something like this. And let's call that one front hub. We should have something like this. This is the basic shape of the gear. We're now going to draw one of the teeth. Let's start a sketch on this large face here. Let's go normal too. First, let's select these two circular edges and then press Convert. And both of those circles should now be added to your new sketch. Then get a sense of rectangle tool and draw sensor rectangle at the origin, something like this. We'll set the width of this as 1.5. So it's the same as the previous gear that we made. Then for the height, you can make this small top line tangent with the outer circle. That should then fully define your sketch. So we can use this for an extrude. Let's just extrude this area up here. So it's just one tooth and it's the same height as that middle section. So it's 2.6 millimeters. You should just have one of the teeth like this, and I'm going to call that gear tooth. We can now use chamfers to angle off the edge of this tooth. Get the chamfer tool, this is underneath the fillet tool on the Features tab. The size of the first one should be 1.5 millimeters, is a 45-degree angle and it's just an angle distance chamfer. Then we can add that chamfer to this outer edge here. Next we'll just chamfer to more riches. These ones are 0.5 by 45 degrees. So get the tool again, set 0.5. And let's just jump at these two angled edges. You should have something like this. That's the first tooth completed. We can then pattern this around. So there's 12 of them. Let's select that gear to feature and also those two new chamfer features. Then let's go to Features, press the drop-down underneath linear pattern, and then choose circular pattern. Make sure you have those three features selected. Will set 12 instances equal spacing 360 degrees. Then clicking this top box for the direction of the pattern. And then we'll choose a circular face. I'm going to select this one. And you should see a preview like this. Make sure you've got 12 instances and then press okay. And we should have added all of those teeth to the gear. Then one of the last things we need to do is cut out the actual hole in the middle of this gear. First I'm gonna start a sketch on the top plane. I'm going to go normal to this actual hole starts like the usual one that we draw. So first I'm gonna get the circle tool. I'm going to draw a 4.8 millimeter circle in the middle. Then I'm going to get a sense of rectangle tool and draw to censor rectangles. They're both the same width, which is 1.8. And for the length they're both linked to the outside of that 4.8 circle using tangent relations. This is the same as the usual actual sketch that we normally draw, but there's actually some extra detail in this one. Let's choose the center rectangle again. Let's draw another sensor rectangle here. There's a little bit longer, and then another one going in this direction as well. Let's make these short edges equal. The width there is 0.85 millimeters, and then the length here is seven millimeters. And that's the same for both of the rectangles. So you can make both of those long edges equal and that should fully define your sketch. It should be something like this. It looks like quite a messy sketch, but we're now going to just extrude certain parts of it. So let's go to Features extruded cut. Let's choose through all both and then clicking the selected contours box. And probably the easiest way to do this is zoom in a little bit and first click on one of the outer lines of those thinner rectangles, and that will select the entire rectangle. Then let's do the same with the second thin rectangle. Click on one of the outer lines, and that will select the entire shape. Initially we should just have this thin crust shaped like this. We also want to extrude the usual actual shape. So let's move around. Let's get this long rectangle bit here with a curved top. It's also that small square in the corner there. And then it's the other long rectangle going horizontal. So for this one it's a horizontal section. It's the corner square, and then it's the vertical section. And then it's the same on the other side as well. You should have a shape like this. And then if we press Okay, that hole will be cut. If I go to a normal two view, you can see the exact shape of it. So it should be completely symmetrical, both horizontally and vertically. If you find that you've missed any areas, you can just edit that cut feature and then you can add the missing areas using that selected contours box. I'm going to call that new feature acts occur. And then the final thing we're going to do is just round off the inner corners here. So get the fillet tool and set at 0.5 millimeter fillet. That's choose these four edges. If you choose the wrong one like this, you can just click it again to de-select. Now we finished the modelling so we can change the color. So I'm gonna go to the Appearance scenes and Details tab. I'm going to choose a medium gloss plastic. And I'm gonna say as green colored. Then I'm just going to save that part. And I'm going to call this 1.5 bevel gear T12 tooth because it's only half the size. And I'm going to put that number on the end, 30465. In the next video, we'll take these new parts and will complete stage 18. 45. Stages 18 and 19: Adding the Tail Section: Welcome back. We're now on stage 18. First, make sure you've got the parts open. We have stage 17 open. We've got the small Bush, we've got the half bevel gear, we've got the friction pain with long axial and we've got the tail rotor. First. We're just gonna make that small sub assembly. I'm going to go to the tail rotor part and then I'm going to go to File make assembly from power. As usual, I'm gonna pin open the insert components menu. I'm going to insert that tail rotor part first. Then that's also insert the friction boom with the long axial. And let's also insert that half bevel gear. We can then just make these together. So firstly, I'm going to select this circular face and this one, I'm going to make those concentric. If you find that your pin is the wrong way round, you can just expand the maze. You can right-click on the concentric mate and you can press Flip Mate alignment. At this stage, I'm also going to lock the rotation because it's quite a stiff pin in that hole. Then I'm just going to drag the pin down a bit and make sure that this outer edge is coincident with this outer edge of the rotor. Then let's do something similar with a bevel gear. So let us select a circular edge. You could select one of the internal edges, but they're very small, low circular ones. So it might be easier to select that main outer circle. And then let's choose a circular edge on the actual. And let's make those concentric. And I'm also going to lock the rotation there. Then I'm just going to pull the gear up a bit so we can see the gap in-between them. Then what I'm gonna do is choose this top face of the rotor here, and then spin around a little bit. Also choose this outer face of that raised part of the gear. Those two should be touching each other. So let's make those coincidence. This is only a very small assembly and we can now save that. And let's call that stage 18. Tend to complete stage 18. Let's go back to stage 17. And then let's go to Insert Components. And let's choose that stage 18 that we just made. We can then insert that and spin it around to the correct orientation. Will also insert this small bush part. Firstly, I'm going to choose this interface of the hole and then a circular face of the axial and make those concentric. We don't need to lock the rotation because we want the blade to spin around in the whole. I'm then going to choose this face and this face and just make those coincidence so they're touching each other. Then let's add the bush to hold that row two in place. So let's select this large outer circular face and also select a circular face on the axon. This concentric mates should be locked because there'll be locked together because of that actual shape. And then for the left, right position, I'm just going to pull it out a little bit. I'm gonna make this outer face of the axial and the outer face of the bush coincidence. We do have a little bit of clearance in there, but that will just help the rotor spin around. And you should find that the tail rotor can spin around within that tail rotor housing. And you can then save stage 17 will now go directly onto stage 19 because it's a very simple one. We've just got to add this stage 18 to the main assembly. Let's make sure we've got opened the main assembly for me. I'm going to find that in my recent documents. And then let's go to Insert Components and choose stage 17. Because remember, stage 17 is actually 1718 joined together. So it should look like this. Let's rotate it around, so it's in this orientation. We can then fix this tail rotor section in place. So let's rotate around. Let's select this pin at the back. Then let's select that second hole from the back on the main body. Let's make those concentric and lock the rotation so that this doesn't move around. Then in terms of the up-down distance, Let's choose this top face of the fairing, then this bottom face of the beam. And let's make those coincidence. We've now got a tail rotor on our helicopter. I think this is looking great. At this stage. You're probably fine that you can't spend the tail rotor around. But this is something we'll fix after we've completed the whole assembly. You can now save your main assembly. And in the next section, we'll go onto stage 20, which needs one new part. 46. Creating the Pin with Large Bush Part: We're now onto stage 20, so we didn't really, well, we've only got three more stages to go for this. We only need one new part. It's basically a pen with a large bush on the end where you can put the excellent. It's very similar to the friction pen. So let's open the friction pen and then let's save this as a copy and make some changes. Go to File Save As, and then choose save as copy and open. And let's call this one pin with large bush. And then you can save it and you can close the original file. Let's make some changes. And if we look at our part, it's actually very similar to this normal pen. It's just got that extra section on the end where the axel fits in. The only things that we need to change on the original pin or the slot curves. So first let's edit that sketch underneath the side slot feature. And we'll go normal too. And we only need the slot cut on one side. Before we delete this slot on the left, then we will lose our dimensions there. So instead of deleting it, Let's select the slot and let's make it for construction. This means it will be ignored by the feature, will only have that slot on the right, will retain all the dimensions in the sketch there. And we can then exit the sketch. And now you can see we've only got the slot cut on one side of the pin. There is actually a slot on the other side, but it's just 90 degrees from that original slot. What we'll do is edit that middle slot sketch. Let's go Normal To, and let's sketch another slot on the left-hand side. Get this lot tool, a center point straight slot, start from the midpoint of this left-hand edge and then draw our slot that's the same size as the middle one. So we can just select both of the slots and we can click make equal. Then let's exit that sketch. And you can see that's locker is now on the end as well as the middle. Basically got one slot on the right-hand side, and then we've got another slot on the left, but he's 90 degrees offset. We can now model up the section on the end where the axle goes in. Now we could make this with a series of circular extrude, but actually in this case it's probably easier to use a revolve. So let's start a sketch on either the front plane, the top plane. It doesn't really matter because it's a revolve. So we can use either one. I'm going to choose the front plane and then I'm going to go normal too. It will start to draw our revolve profile. Because it's a revolve. I'm gonna start with the center line that we can revolve around. Get the center line, Let's go out from the origin to the side horizontally. Then just get the line tool and let's draw something like this. It's a profile that's kind of wider at the end and then it's thinner in the middle and then wider again. Then there's a little wide section here on the right and then go back to the middle and then close the profile. This is basically a cross-section of the area where the actual face into. Now we can start to add some dimension. So let's get this Smart Dimension Tool. I'm going to start with this left-hand edge. If you find that you try to add a dimension between lines and you get an angle instead of a distance, then it just means that the lines aren't parallel in this case and need to make sure that that center line is completely horizontal. And then I'm going to start to add the actual sizes. I'm going to click this line on the left. I'm also going to choose the center line. Now you can see we've got the dimension between those two lines following the mouse around. We could click to place this, but before we do, we're actually going to move to the other side of the center line. This will automatically double that dimension. It will give you a full diameter dimension. Instead of just a radius. We want to add that dimension, but then move over the center line before you place the dimension. Then let's set this to 7.4 millimeters. So it looks like this I mentioned is just floating in space. But actually what it's showing is the full diameter distance there. So it's the distance to the center line and then the same distance again. And then moving on the length here is 1.4 millimeters, the diameter here. So let's click on the line. Let's choose the center line. Let's move to the other side of the center line. And then let's set the diameter there as 5.7. Then this diameter here on the right should be 5.9. And the length of this part on the right is 0.8 millimeters. Will then select these two lines and make those co-linear. They are spaced out at the same distance. Will also choose those two lines again and we'll make them equal. So that makes them the same length, 1.4. And now to anchor the position in space so we know the total length of the pin from one side to the other should be 23.7. So I'm gonna write that in. Then finally, we know the distance inside here should be 5.1 millimeters and that should fully define your sketch. Overlaps the end of the pin a little bit like this. We can now use this profile to do a revolved Boss Base. So let's go to Features revolve boss base. And you probably automatically get a preview. That's because we've got a center line in the model that's automatically being chosen as the axis of revolution. If you can't see the preview, just click in this box up here on the left, and then make sure you have that center line chosen for the axis of revolution. And we want to revolve 360 degrees. We've got preview. Looks good press. Okay. And we've now added that new section on the end. And you can call that feature something like large bush. Now we need to cut out the actual shape in the middle. So let's start a sketch on this end face. Let's go Normal To, and let's draw our usual actual shape. You might be happy to hear that this is the last time we're going to have to draw this. There's a circle at the origin, that's 4.8. And then it's o2 sensor rectangles that are the same width, 1.8 millimeters. And then the length of them is set by that 4.8 circle using those tangent relations. When you've drawn it, let's go to Features extruded cut. Let's just choose those five areas in the selected contours. And then for the end condition, we don't want to cut all the way down here. We actually only want to cut to this face on the inside of the rim. For the unconditioned, let's choose up to surface. And then for the surface, Let's choose the end surface there. We're just cutting inside that wider bit. That's why we've got that little rim on the end of the revolve that we had it. Let's press Okay, and let's rename that as axial cut. Then finally, we just need to add the slotting on this end. Let's start a sketch on the front plane. Let's get the slot tool and a center point slot and draw a slot in this kind of position. The length of this slot should be 4.8 and you'll have to hold down Shift to dimension to the outsides of the arc. The thickness of it is one millimeter. And then the slot should be lined up horizontally with the origin. So if yours can move up and down, then just select the center point of that slot. Also select the origin and press make horizontal. And then from the end here, we know that it should be half of 5.1, so it's 2.55 millimeters, then that should fully define your sketch. So you can go to Features extruded cut and we can go through all both. And let's call that feature at Bush slot. Then let's just change the color to that sort of light gray color. Then this part is complete and you can save it. In the next video, we'll use this part. So complete stage 20. 47. Stage 20: Starting the Skids: We're now onto stage 20. And this is quite a fast one. It's got a really small sub-assembly with just two parts. We could just add these directly to the main assembly, but instead we're going to follow the process that we've used all the way through. Make sure you've got open that new large Pim with brush that we just made, and also the cross block. You can then go to either one of those and choose File make assembly from parts. Then I'm going to pin the insert menu open. I'm going to choose that crosswalk file. And I'm gonna insert it fixed to the origin of the assembly. Then I'm also going to insert that pin with large bush. Let me can mate them together using a concentric mate. So choose to circular faces, one on each part and make those concentric. You don't really have to lock the rotation for this one because it could spin around. But what I'm gonna do is choose this face and this flat face. And I'm gonna make those parallel just so that the final axons that make this kids at the helicopter aren't wonky. Then let's just choose this face and this face and make those coincident. So you should have something like this. It's a very simple sub assembly. We can then save this as stage 20. Then let's go back to our main assembly and let's insert this new server assembly. I'm going to spend my model around and start on this side first. So I'm gonna go to Insert Components and find stage 20. And then I'm gonna spin it around and I'm going to put it roughly there. The bushing part where the axle goes in to be facing to the front of the helicopter. Then let's just move it to about the right position. And let's choose a circular face here and also inside here. And then make those concentric. And I'm going to lock the rotation. Then let's choose the outer face of the Bush and then the corresponding face on that cross block part. And let's make those coincidence. We should have that one's good holder on the back like that. Then if we look at the instructions as also actually another cross block on the front, that's just a single part. What I'm gonna do is hold down Control, going to left-click and drag from this cross block at the back, and then release the left mouse button to insert a copy of that part. We can then make it in place. I'm going to make these two circular faces concentric. I'm going to lock the rotation. And then like with the one at the back, I'm going to select the outside of the bush and the other side of the cross block. And I'm gonna make those coincidence. We've added the two ***** holders on one side. We also have them on the other side. We can mirror these over. So let's go down to the bottom of the parse tree and let's edit our mirror components feature. You can click on this and press Edit Feature. Then in his components, the mirror box, Let's choose firstly that new cross block and then also that sub-assembly at the back. You can click on either part and it should say stage 20. Then we can press Next, and the preview looks good. So let's press. Okay. We've now added those get holders onto the other side as well. We'll finish those kids off in the next section so you can now save your main assembly. 48. Making the Light Stud and Pin with Stud Parts: We're now on the second-to-last stage. And for this, we've got to make two new parts, but they're both very simple, so we'll make them in one single video. We have to make the light cover stud and we have to make the pin with a start. We'll start with opinion withstood. And this is very similar to one that we've already made. That's this one at the end, the pin with the axial. Let's open that friction pin with axial part and then save it and make some changes. So it should look like this, but instead of the axial here we want to add a little stud. Let's go to File Save As, and then choose save as copy and open. Let's call apart friction piton with start and then save it. Then you can close the original document. Instead of an axial here on this side, we just need a small study you can put a brick onto. Let's delete the last three features. They are all the features related to the axle. You can also delete the sketches that are underneath them. And then all we have to do is start a sketch on this interface. Let's choose the inside circular edge and press Convert. Then let's open the circle tool. I'm going to go normal too, so it's a bit clearer. I'm going to draw a circle at the origin. The outer diameter of that is 4.9. And then we just need to do a blind extrude with this. The height of that is 1.8 millimeters. So press Okay to add that stuff. That's it. That's all there is to it. So let's just change the color of the spot. Let's go to the Appearance scenes in Details tab, and let's change it to a blue color. And then finally, I'm just going to rename that latest feature as stirred. And then you can save your part and we'll go on to the next one. That's a little stud that fits onto the end of this pen. Let's start a brand new part. This is a very simple one as well. It's only got two features. The first one is a revolve, so let's start sketch on the front plane. Let's get a center line and draw a center line from the origin directly upwards, vertically. Then get the line tool and draw something like this. Start at the top point of that center line and go out to the left horizontally, then go vertically down, almost all the way down. So you're in line with the origin, but not quite that far down. Then go a little bit over to the right-hand side horizontally, then go directly down to the origin. And then in a little bit more, and then go upwards, then in back to that center line, and then go back up to the start point. Then when you've got a closed profile, we can start to add some dimensions. The main outer diameter is 7.8 millimeters. To add this, select that vertical line on the left-hand side, and then select the center line and then move over to the other side of the center line. And we can add that full diameter distance. That should be 7.8. When you add that first I mentioned it should resize the entire sketch. Then this inside diameter here is exactly five millimeters. This little step-up here is six millimeters diameter. And then the height of that step is 0.2. So it's just a tiny little step. They see inside lengthier is 2.1. Then the total height from the very bottom is 3.1. That should fully define your sketch. If you're not fully defined, then just make sure these lines at the bottom or horizontally inline with the origin. Then let's use this profile to make a Revolve Boss Base. So let's go to Features revolt boss base. You should automatically get that preview because we've just got that center line that we're going to revolve around. If not, you can choose that center line as the axis of revolution. And we're going to revolve all the way round 360 degrees. And then it should look like this. It's a very simple part. I'm going to rename that feature as main body. Then there's just one more feature inside the capsule. We're going to spend the part over. I'm gonna start a sketch on this inside face. Select that face and then press convert entities. We've now made the outer circle of the face into a new circle in this new sketch. Then we can get the center rectangle and draw a rectangle at the origin, just make it a little bit bigger than the circle like this. We're going to set one of the sides as 4.8 millimeters, then the other side should be the same length. So choose those two sides and make those equal. So we've got a square that's 4.8. And this just gives a little bit of grip to allow these parts of grip onto Normal brakes and onto that pin withstood that we've already made. We can now go to Features extruded boss base and in the selected contours, Let's just choose these very small wedges in the corner. There should be four of the main total. For the depth, you can choose up to surface. And then we can choose that very bottom surface. So this just makes the inside a little bit narrower to allow it to fit onto the other breaks. So let's call this gripping ribs. Then to finish off, let's just change the color. So let's go to appearances which use a Medium Gloss red plastic. And then you can save your part. And let's call this one light stud 30465. We now have both parts that we need. And in the next video, we'll go into stage 21. 49. Stage 21: Finishing the Skids and Tail: Stage 21, the second-to-last stage. We're going to make that little sub-assembly first, make sure you've got opened the friction pen with stud and also the lights did that we just made. Then go to either one of those parts and let's go to File make assembly from part. You can pin the insert menu open. And first let's insert the friction pyramids stood fixed to the origin of the assembly. And then let's also insert the light stood. We can then make these in place. So let's choose a circular face on each one and make those concentric. And if you find that your stirred spins the wrong way round, you can just expand them mates. You can right-click on the concentric mate and you can press Flip Mate alignment. I'm also going to lock the rotation of this. We probably don't really need to do this, but it's just for completeness. Then I'm just going to select this face on the Penn and his face on the stud. Join those together using a coincident mate. That's this. So assembly finished a very simple one there. Let's save this and let's call it stage 21. Now we can go back to our main assembly and we can add that mu sub assembly to the main one. Firstly, looking at the instructions, we need to flip the model over and we need to spin it around. We should be looking from this kind of view. Then let's go to Insert Components. Let's choose that stage 21, unless insert it somewhere around here. Then let's just zoom in and let's add a concentric mate by selecting those two circular faces and making those concentric. And I'm going to lock the rotation as well. Then let's just move this part into position by selecting, say, this inside face here, and then the corresponding face here, and making those coincidence. So you should have that light stood on the back of the tail rotor there. And that's just the navigation light on the back of the helicopter. To finish off this stage, we also need to add the skids. These are made from the axial part. Let's find an axial already exists in the model. Any of the axons will do. Then hold down Control, left-click and drag from an existing axial, and then release the left mouse button. And that should insert a new copy of that part. The axons that we want our six long. So I'm gonna click on the part and then from the configuration dropdown that should appear. Let's choose six long. We can now make this in place. Let's zoom in a little bit. Let's choose a circular face on the axle and then the corresponding circular face on one of the good parts. So it should look like this. Now if you find that you're actually is misaligned with the axial hole, then you can just drag out a little bit, choose a flat face on the axle and then a corresponding flat face in the actual hole and make those parallel. Then for the actual depth of the axial, Let's spin around and let's choose that face in the very back of the axial whole. So it's the inside cross face and then spin around and also choose the end face of the axle. And let's make those coincidence. That should pull the axial back to the correct distance. And then there's just one more on the other side that's the same position. We can use our mirror for this. Let's go down to the very bottom of our part string. I'm just going to minimize the sub-assemblies to make it a bit idea. And then click on the mirror components feature and press Edit Feature. Then in the components, the mirror box, let's just select the actual that we just added. Let's press Next. And that preview looks real good too. Let's press. Okay. We now have the axons that make up the skids on both sides. We've also got that light on the back. Stage 21 is complete. We've only got one more stage left. And for that we've got to make those all important rotor blades. 50. Making the Main Rotor Blades: We're now on to the final stage, stage 22. For this, we've only got to make one new part, the main rotor blade. To do this, we're going to modify the large bush part. Let's find that part somewhere within the assembly and open it. And then let's go File Save As, let's choose save as copy and open. Let's save this as large rotor blade. You can then close your original part. If we look at the rate of labor on the right, it's a large bush and then there's sort of a pin area, and then there's the actual rotor blade. We can keep this large bush part exactly as it is. We don't have to take anything away. We're just going to add some new features. First, let's start a sketch on the right plane or go normal too, and get the circle tool and draw a circle somewhere down here. It should be the opposite end to where those scallop cuts off. Then the diameter should be 7.4 millimeters. And there's also a smaller circle inside this one, this 4.8 millimeters. They should both be lined up vertically with the origin. And then for the position from the very end here to the outside of the circle is 15.6. And you can hold down shift to dimension to the outside of that circle. You should have to fully defined circles which are a little bit away from that existing body. We can then go extruded boss base. Let's go mid-plane, 7.8 millimeters. And that should insert a new body like this. And we can call that something like pinhole. We now need to join these two bodies together. So let's start a sketch on this face, on the first body. And then let's select the outer circle and press convert entities. We should have a 7.4 millimeter circle. In this new sketch. We can then just go extruded boss base. And from the drop-down, let's choose up to surface. And then let's select this surface. You should join these two parts together, something like this. And we can call that feature join. Next before we start actually making the blade, Let's cut out the small rim on the top of this pinhole. Start sketch on this top face. Choose the inner circle and then just offset that 0.7. We can then do an extruded cut downwards 0.8. You can call that feature something like REM cut. We now have the outer rim on one side and we also want it on the other side. So let's select that rim cook feature. Also select the plane that goes down the middle and then press mirror. And when the preview that's good. Just press. Okay, so we have that rim cut on both sides. Now we can start to actually make the rotor blade shape. First that we've got a bit of a root section that's a little bit wider than the main blight. To draw this, Let's start a sketch on the right plane and go normal too. Firstly, I'm going to select the outer circle of the pin area and press convert entities. So we now have that circle in this sketch. Then get the line tool and draw a profile, something like this. From this outer point of the circle, I'm gonna go directly down and then directly across. And then I'm gonna go upwards and slightly right, so we've got a little bit of an angle and we're going to join that circle. So we don't want to go up vertically. We want a little bit of an angle like this. And let's join on that circle somewhere around here, that, that widest point. We can now set some sizes. So let's set the total height here as 25 millimeters. The width across here should be 6.4. Then over here, let's just select the circle, also select the line and just make those tangent. And that should fully define your sketch. And then just before we extrude, Let's just round off these bottom corners. I'm going to go to the Sketch tab. I'm going to choose sketch, fill it, and then set a size of one millimeter, and then just select those two bottom corners. We can now extrude this closed area. So let's go to Features extruded boss base. And I'm going to choose that area there. And then we'll do a mid-plane extrude three millimeters. You should have something like this. It's like a really small section of the blade. Let's call that feature blade root. We can now draw the rest of the main blades. So let's start another sketch on the right plane. Firstly, again, let's zoom in and let's select this circular edge and press Convert. You can either select the full circle or just that bottom edge. I've just selected the bottom edge. Then I'm going to get the line tool. And from this left-hand corner I'm going to go all the way down vertically about that. And then I'm gonna go in at an angle, and then I'm going to go horizontally across and then vertically up to about here. And then into this angled line. And make sure you don't get the midpoint. We should be somewhere above it about here. Then I'm going to get back into the right-hand point of that circle. You should have a fully closed profile, something like this. Then let's set the size. So the total length here from the very end should be 63 to this small end section here is 4.6. The length of this angled part is 11. And then going up to this corner from the very end here to this part should be 15.6 millimeters. The lengthier should be 4.5. And then finally, the total width of the blade should be 11.2. And that should fully define your sketch. I'm just going to rotate it around so it's a little bit clearer for you to see. We can then extrude this using a mid-plane extrude, Let's go to Features. Let's do a mid-plane, two millimeters. If you selected that full circle on the right-hand side, you might just now have to click in selected contours and choose that and closed profile for the blade shape. But we should be extruding two millimeters mid-plane. You can then call that feature blade. Now before we round this off, there's a slight edge on the back of the blade. So for the airfoil shape, and we'll make this using the chamfer. First select the chamfer tool is underneath the fillet tool. And for the chamfer type, we want to choose distance, distance, not angled distance. If you're on a different version of SolidWorks, your interface here might look slightly different, but they should still be an option called distance, distance. Let's select that one distance distance. And then down here at the bottom, instead of symmetric where you want asymmetric. This just means that we can make a chamfer that isn't symmetrical. Each side of the angled cut will be a different length. For those two different lengths, we want to put 0.4 as the first one and then five millimeters as the second one. And then let's select that trailing edge of the blade like this. You should get a preview like this if yours doesn't work or if it looks like it's the wrong way round, then try just flipping that 0.45 millimeters on the left. So try putting five millimeters in the first box and 0.4 in the second one. Then let's also select this bottom edge. If you find that you can't select both edges, then you might need to add this feature as two separate chamfers, but it should work correctly like it does in this video. Then let's add those chamfers. And we've just added a slight sort of airfoil shape to the back of the blade there. Then let's get the fillet tool and let's round off that chamfer. I'm going to add a very large fillet, 50 millimeters to this edge on the top and also the same edge on the bottom. Next we can round off some of the outer edges. So I'm going to get the fillet tool again, this time set to millimeters. And let's choose 123 edges. Then on the corner at the front is a bit of a larger one. So let's get the fillet tool again. This one is 20 millimeters and it's that front edge there. And then to finish off, let's get one final filler. Set 0.5. And let's just add the front edge there. You should select the entire way round automatically. Let's also do the same on the bottom. If you find that you don't select the entire loop, just make sure you've got the tangent propagation option selected on left and then press OK. And there we have our large rotor blade and you can keep the color of the same. In the next video, we'll add this to the final stage. 51. Stage 22: Finishing the Helicopter and Adding Mechanical Mates: Welcome to the final stage. In this video, we're going to add the rotor blades to finish off the model. We're also going to fix some of the colors that are a little bit off. We're also going to add the final mate so that the blades and the tail rotor work together properly. Firstly, make sure you've got your rotor blade part open. And from within the main assembly, let's go to insert components. Let us choose that rotor blade and just place it in the main assembly. We can then make it in place as usual. So let's select a circular face on the blade and also on the axle that goes through where the blade attaches. Let's make those concentric. And you can lock the rotation as well. And then I'm just going to zoom in. I'm going to select this face and the corresponding face on the blade, and I'm going to make those coincidence. Then we want to add an opposite blade on the other side. To do this, I'm just gonna hold down control and left-click and drag from that existing blade and then release the left-click and that should insert a copy of that blade part. Then I'm going to rotate it around by holding down the right mouse button and just rotating the part. And then we're going to select a circular face on the axle and also a corresponding face on the blade. And I'm going to make those concentric. I'm going to lock the rotation. But first you might have to just move it to the correct angle. So I'm going to select two flat faces and just make those parallel. Then I'm going to select the interface of the blade and the outer face at the hub and make those coincident. There we have our finished helicopter. We've got all the parts all assembled correctly. Now, you should find that you can spin the blades around like this. However, to fully finish, we need to add some mates so that when you turn the main blades, it also turns the tail rotor will do that in just a moment. But before we do, if we look at our model, we can see that the green colors don't quite match up with each other. That's because I just added these by eyeballing the color as we went through. I didn't make sure that they were the exact same color, but now we've got all the parts together. We can see there's a bit of a mismatch. I'm just going to edit some of those colors. Now you don't have to do this, but it just makes the model look a little bit better. So from within the assembly, I'm going to go to the Display Manager tab. And we can see here all the different colors of all the different parts of the model. So firstly, I'm going to find one of the greens that looks correct, that looks close to the actual real-life par. I think this fairing part of the back looks probably the closest. Here on the left, I'm going to click on the green parts one-by-one. And I'm going to find that tail fairing part. You should see as you select the different green colors on the left, you get a very faint box around the parts in the main assembly. And I can see when I select this one on the left, that is actually the tail fairing on the right. You see it's got that very faint box around it. Now we have the correct ones selected. I'm going to edit that appearance and find out exactly what the color is. Let's right-click on the parents and press Edit appearance. And then if you scroll down to where it says color, we can see the color that's selected. And down here we can see the RGB value. This is a numerical value that tells you the exact color. So we can see it's 177 red, 255 green, and eight blue. I've now made a little note of that, of the color value, and I'm gonna close this color. We can then edit the other colors and we can change them to match this exact color. One-by-one. I'm just going to edit the different greens in the model and I'm going to change those values. As I said, you don't have to do this, but it just makes them modal look a little bit more standardized and a little bit better. I think one-by-one, just edit those appearances and go down and change the value to the one that we just wrote. So it's 1772558. Now this is a little bit tedious and you can see that it probably would've been better if we did it as we went through. But there's only about four or five of them that needs to be changed. And you might find that yours are very close anyway, so you don't need to do this. When you done, we should have the same green in all of the parts. We're now going to add the Mechanical Mates so that the blades and the tail rotor work correctly together. Firstly, we've got the main rotor that moves around. And then we've also got this transmission part that goes along the tail. The first thing we need to do is just line up the gears so there's sort of meshed together properly. Zoom in a bit. It's kind of hard to see, but we want to move the gears around. They're not actually clashing. There's a small gap between them. So hopefully you can see that I've moved them around so they're not really overlapping each other, but they're lined up correctly. And it doesn't matter too much if you are a little bit off, it's mainly just for visuals. We can now add the Mechanical Mates between the two assemblies. To do this, let's go to the Assembly tab and select the mate tool. Now we need to choose the mechanical mate section. So click on this mechanical tab. If you've got a different version of SolidWorks, you will lay out might be slightly different here. You might have to scroll down to the bottom and you might find the Mechanical Mates down there. But within the Mechanical Mates, we're looking for gear mate, which is this one. Select that gear mate. And the first thing we need to do is choose two different selections. These are basically two different gears. I'm gonna make sure I'm in that mate selection box on the left. We want to choose two different circular faces, one on each sub assembly. So one of the main rotor blade and worn on the transmission. For the first one, I'm going to zoom in. I'm going to choose this bush here, which is on the transmission of assembly. We've selected that bush and basically we've selected that whole assembly. Next step we need to choose another circular phase, which is on the rotor blade assembly. I'm going to zoom in. I'm going to choose this one up here. We have two circular faces selected, one on each subassembly. We now need to set the gear ratio. This determines if we turn the rotor blades once, how many times will the transmission turnaround? If the gear ratio is the same and the rate of lights turnaround once than the transmission will also do one revolution. So it will also turn around once. Now if we look at the two gears, they're actually the same size. So we do want that one-to-one ratio. If, say this gear at the back was twice as big, then you might want to have a different ratio, two-to-one. Here on the left, we can set the ratio. And if you've selected the same selections as me, then you probably get the same ratio of 5.75.7. And this is based on the diameter of the faces that I selected. If you made a different selection, then you might have different numbers in there. We need to set a one-to-one ratio. But actually your 5.75.7 is a one-to-one ratio. As long as those two numbers are the same, then it will be a one-to-one ratio. So make sure that those two numbers are the same. If you select a different faces than maybe just change it to one-to-one and then press Okay to add that mate. Let's have a look and see if that works. I'm gonna try and spin around the main rotor. And you can see as I turn it, it does actually turn that transmission at the back. If I zoom out a bit, it's a little bit easier to spin it around. You can see that is working. However, if you zoom in and you have a look at your gears and you find that one of them seems to be turned in the wrong way round. You see as I turn this gear, the other one seems to be turning backwards. What we need to do is just reverse the gear mate. If you're still in the main tool, you can select the meat down here and then just press reverse if you're not in there make tool, Let's just zoom down to the bottom, expand their mates folder. Then let's edit that gamete. So let's go all the way to the bottom. It should be the latest one. You can right-click on it and you can press reverse. You can press Edit mate. And then from within the property manager, you can click the reverse box here. I'm going to press reverse and then press Okay. Now you should see when you turn the kids, they mesh together properly. We've done the main blade and the transmission. Now what you also want to add the tail rotor before you actually start to add the Mates here, Let's just try and manually spend that tail rotor around. So just left-click and try and drag the part around and see if it works. And you'll probably find that you can't actually rotate it. You get a message saying that it's fixed. That's because this tail rotor is actually a sub-assembly and by default, subassemblies are inserted as rigid. So that means the parts within them can't move within the larger assembly. But luckily, it's pretty easy to make these subassemblies flexible. What we need to do is finally, appropriate sub-assembly should be staged 17. And then click on it in the pot straight. And then from the pop-up menu, Let's just choose this option. Make sub-assembly flexible. I'm gonna click that and you can see now here on the left, the icon has changed. You can see for example here stage 21. This is a rigid assembly, this kind of icon. And then a flexible assembly is a slightly different icon here. Now if you go to the graphics area, you should be able to spin that rotor around just by dragging it. We can now just add the second game ate in the same way as we did with the first one. Firstly, let's rotate our parts around so they're meshed correctly, so they're not overlapping with each other. Then we can start to add the gear mate. So I'm gonna go to the move tool. I'm going to choose Mechanical Mates, and I'm going to choose gear. Then I'm going to choose a circular face on the transmission of assembly, for instance, this one on the axle, and then also a circular face on the tail rotor sub-assembly, for example, this one on the hip. Now you can see because I chose parts that are different diameters, we have a ratio that's different here in the property manager, but we actually want a one-to-one ratio as well, because both of these gears have 12 teeth, so they should move together at the same rate. In these boxes on the left, I'm just going to change it to a one to one. If we just try and rotate the parts around, I can see that that the gears on machine backwards. I also need to reverse the gear mate. I'm just going to line them up again and I'm going to click that reverse box on the left. Now we should see that they're meshing together properly in the correct direction. I can press Okay to add that gear mate. You can then close the shop. Now if we zoom all the way out, we should see that when we turn the main rotors, it turns the tale writer. That shows we've added the gametes correctly, well-done, this assembly is completely finished. We built all of these parts from scratch and we made it work in Lego helicopter. At this stage, you can save your assembly. We're completely finished. If you want, maybe you can make another assembly using the same parts. If you do, please upload a picture of your design by completing the assignment in section. That assignment is completely optional. You don't have to do to finish the course. If you're sick of Lego, you can finish here. Thanks for taking the course. I hope you enjoyed it and you maybe learned a little bit or practice your SolidWorks skills. I hope to see you again, maybe you're on future courses. Thanks.