Learn Fusion 360 - Complete class for creating Assemblies

1. 01 Introduction: Hi, I'm Ja Haru. I'm a Fusion 360 certified user and Auto Dec certified professional. I have over ten years of industrial exposure, especially in design field. I will be your instructor in this course. I will be teaching you about making component assembly in fusion 360. In this course we will start with some basic assembly, then we will make some intermediate assembly, and finally we will learn some advanced ones. Now if you are a complete beginner to fusion 360, this course might not be for you. You need to have some fundamental knowledge of two sketching and three D modeling. 2. 02 How to download Fusion 360 for FREE: Now the very first step would be to download Fusion 360. Now for that, we are having two options. Either we can download Personal Use license or we can download educational license. It depends if you are a hobbyist then you must download the personal use license. Or if you are a student or educator associated with the education institution, you can download educational license for both of them. I will be showing you a walk through now for downloading personal users license. This particular link is there. You can utilize this link. It is also available in the resources for educational license. This particular link is there now for both of them. For both the license, you need to sign in or you must create a auto Dex account. If you already have a Autodex account, you can just select next over here. Or you can create a account by clicking here and providing your details. I already have account, so I will be just moving forward now. As soon as I have signed in, I can download Fusion 360 for personal or hobby use. Just have to click here and get started, then fill on all the details and your download link will be available. Now for the second version, the second variant educational license here also you have to sign in first, then you have to click on Get Started. You can also watch this video of how this educational license works for the sake of better understanding, let's just click here. Then it will again ask you to sign in. Then you will be asked to confirm your eligibility for educational access to this Autodex product, not only Fusion 360. You can download all this Autode product if you are a student or educator. This is the main difference between a personal license and educational license. With a personal license, I'm only able to download Fusion 360, but with a educational license, you have a library of softwares of Autodex. Here you have to click on Get Started. Then you have to provide identity proof of your educational institution. These three documents regarding your legal name, the name of your education institution, a date within the current school term. This does not falls in my category because it's been a decade since I have passed my engineering. This will not be applicable to me. I will be using personal license only as soon as you have downloaded the software. For personal uses, it is you will get this message, personal, not for commercial use. 3. 03 A brief revision of commands: I assume you must have downloaded the software by watching the previous lecture or you must be already having Fusion 360 installed in your system. Now, as explained in the course description itself, this is not a beginners course, it's a intermediate course. You must have some fundamental knowledge of two D sketching and three D modeling in fusion 360. But in case, if you just want to learn the component assembly of fusion 360, there is a way for that. In this particular lecture, what I'm going to do is to revise certain commands that are going to be used quite frequently in the course. In that way, even if you are a complete beginner to Fusion 360, you can still create the assemblies that I'm going to show in the court just following my instructions. But my recommendation would be to get some insights of two D sketching and three D modeling of Fusion 360. Let's begin now. The very first thing in creating a three D model and creating an assembly, and creating anything in Fusion 360 is to start with creating a sketch. Whenever we click on Create a Sketch over here, you'll be asked to select any one of the plane. Let's select this vertical plane. Then you can see we have a bunch of commands inside this create tool bar, and then in modify, and then in constraints. Let's discuss them one by one. And I'm not going to explain each and every commands because that will take a lot of time. I will be explaining the commands that is being used in this course quite frequently. In this regard, the very first command is line. The shortcut for the same is L in the keyboard. As soon as we invoke that, you can freely create line anywhere in the sketch plane. Next we have rectangle. The shortcut for invoking rectangle command is R in the keyboard. As soon as we invoke the rectangle command, you can see in the sketch pellet. You can have feature options here. You can select two point rectangle, three point rectangle, or a center techtangle. This center rectangle will be used quite frequently in the course. Let's go with this one. You can create a center oriented rectangle. Next, we have circle command. The shortcut for the same is in the keyboard. As soon as we invoke the circle, we have five types of circles. In the catch ballet, we will be using this centered dimeter circle quite frequently. For this, you have to just specify a center point, and you can just drag the mouse outwards and you can specify the dimensions. Your circle will be created at any point. If you want to cancel the command or get out of the command, you have to just press Exit in the keyboard. If you want to repeat the same command, you have to right click and you will have this mark up menu, this radial one appearing. From here, you can repeat the previously used command. Just press exit. Now, next arc three point will be used quite frequently in the course. Let's understand this. For this, you need to select first point, that is the start point, then you have to provide the end point. The third point, this is a three point. The third point will be the deciding point for its curvature. Next slot, we'll be using this one center to center slot quite frequently. For this, you have to provide first point, then the center point, second centerpoint. And you can directly create a slot. It will automatically maintain tangency. This sign, this omega like sin, is for tangency constraint. Next we have this mirror command. For this, we need a mirror line and the objects. Let's say I'm selecting this circle, and for the mirror line, I'm selecting this particular line. It will create a identical one in the other side. It's like creating a mirror image. Then we have this circular pattern. This basically duplicates the sketch entities in a circular way. For this, let's say I'm selecting this arc itself, and for the center point, I'm selecting the center of the circle. It will create multiple number of sketch entities depending upon your requirement. Let it be three. Only. As soon as you're finished with the sketch, you can just click Finish Sketch. You can left click, drag the mouse and select all the things you don't want, and you can just simply press delete in the keyboard. If you want to edit any feature, you can edit it from this particular time line. Let's edit this sketch from where we have deleted. Now here self, let's create a line. Now if you want this line to be tangent to the circle, you can use this tangent constraint line, the circle and the tangency will be maintained automatically. Now let's say I have another line somewhere over here. You want this line to be equal to this line, so you can utilize the equal constraint like this and it will be equal like this. There are many constraints that you can play around with. Often this tangent constraint is used. I have explained that one yes. One more thing was remaining, that was trim command, The shortcut for the same is in the keyboard, you can just invoke the command and you can trim any unwanted portions of the sketch. One more thing was there, let's say these two lines are there and you want to create a fillet in between, you can simply invoke the fillet command from the modified toolbar, provide a fillet. In the same regard, we have offset command, the shortcut for the same is in the keyboard. Or you can invoke it from the modified toolbar over here, and you can create offset of anything. As soon as our sketch is completed, we can create a three D model out of it. For that, you have to just select a Sion, right click, press pull, and you can provide the distance up to which you want to T. This can be one side, this can be two side, or this can be symmetric as well. All the sketch creation, three D model generation, all of these things are happening in design work space only. This course is completely revolving around design work space only. Now here, when talking about three D modeling, we have different set of things. We have lots of, lots of commands over here, out of which we must know about revolve and up to a certain extent, these pre made entities like box cylinders, sphere. And now, before explaining this three D modeling, let's step back a bit and understand the canvas selection. Now this pan movement is being done by pressing and holding center mouse button. Zooming and zoom out is being done by scrolling, scrolling the center mouse button. This orbit is done by pressing Shift plus holding the center mouse button at any time, if you're losing focus of your sketch, you can always click on this home button in the View cube. This is the view cube where you have top, front, right view, and isometric view. Also, if you want your sketch to fit, always click over here or you can zoom window like this. Now coming back to the three D modeling, we understood about the trot feature, the press pool feature. Now is the time to understand about revolve, which is also used in the course. For that, we have to create a sketch in any of the plane. Let's invoke the line command and just create something like this and finish the sketch. From this profile, we are going to create a revolved component or revolved object. Go to Create Toolbar. Click on Revolve. This profile is already selected for the axis. Select this one and see this is Water Revolve Commanders. Now here we will understand some modification tools like Fillet. The shortcut for the same is in the keyboard. You have to select the edges and you can drag this handle to provide the fillet. Click on. Okay, now on this particular model, you can select this face and let's create a rectangle anywhere. The shortcut for creating rectangle was what are in the keyboard. Finish the sketch and select all the profile. Right click, press pool, just like a new body operation. You can also have a cutting operation using press pool. Let's create a circular pattern. Now here we have four types, faces, bodies, features and components. This cut that we have created right now, it's a feature select feature. Let's select it from the timeline for the axis. We need axis on this particular body. For this, we have this construct tool bar from which we can create axis through cylinder, cone, and Taurus. Let's select this one. Okay? And the axis will be created. This construct tool bar will be also used quite frequently. We will be coming to this one also. Now, since this axis is created, we can create the pattern. Let's go to circular pattern from the create tool bar for the object. Let's select feature. Which one? This one from the time line. This cut that we have created for the axis. Let's select this axis. Let the quantity be three only, and click on Ok. This is how circular pattern in three modeling works. Now coming back to this construct tool bar, we will be using this tangent plane and this plane at angle and this mid plane quite often for the tangent plane, as the name suggests, you can create a plane tangent to any conical phase, just like this. Over this, you can create a sketch. This comes very handy when you want to create a hole, a thorough hole, through a curved surface. Let's create a sketch on this one. Let's finish the sketch. And you can see that it has been created on a curved surface and you can create a clean cut hole. The next command in the line in the construct tool bar is the mid plane, and it creates a plane between two surfaces. Lastly, we have this inspect tool bar from which we can measure certain distances. Here you have to select one of the objects. It can be a face, it can be a edge, it can be a body. You have to select another one, and you can see its distance as you can see here. With this, I assume that you got a brief revision of commands in fusion 360. Even if you are a beginner still, you can go forward in the course. 4. 04 Top down design concept: To better understand the assembly making process in Fusion 360, you should first understand the two common types of assembly structures, That is bottom up assembly and top down assembly structure. Let's first take a look at bottom up assemblies. This is the most traditional assembly modeling technique. If you are a user of Autodex inventor, solid works, or any other Cat program, then you must be already familiar with this one. The essence of the bottom up assembly technique is that each part or component is created as an individual file, which we generally call as part files. And then all of these part files are inserted into one assembly file where the parts or components are constrained to each other. With this method, most programs do not create a direct link between these parts. If the parts are required to fit together, then you will have to make sure that you design them to the appropriate size before inserting them into the assembly file. If you make a small change in the part, other part will be affected and you have to make sure that you go back and update those affected parts accordingly and then reinsert them into actual assembly file. On the other hand, we have top down assemblies. The top down technique means you start with an assembly file and build all your parts or components within the context of the assembly. Parts can be built in place and can reference each other, making these parts capable of automatically adapting when you change size or location. Fusion 360 falls into this top down assembly category. Now to better understand this top down approach, let's take an example here. As you can see, there are two components which constitutes assembly. And they are joined together with a rigid joint over here. Now, these two components, these two parts, they have not been imported from anywhere. They are made here itself. In this assembly file, there is just one file, a singular file. This assembly file in which this component and this component is located. That is the first thing that makes a top down assembly a new choice for designers. Now, for the second thing, we have adaptability. If I change anything in this particular assembly, in any of the component, the other component will follow. Let's say we are changing this sketch. We are making the circle a bit shorter, as you can see the other component followed and adapted. This adaptability is the second most important thing in top down assembly structure, which makes fusion 360 a choice for the new age designers. With this lecture, you got the idea of the top down design approach of Fusion 360 from the previous lecture. You got to know about the frequently used commands in this particular course from the very next lecture, we're going to start with the assembly making process of fusion 360, starting with the difference between bodies and components. 5. 05 Bodies Vs Components: Now here in this assembly, there are four basic entities. This Cam, the pin that is attached with the follower, and the pin that is attached with the Cam. These four entities are what we call components in feet and 360. These components are what that makes a assembly. Now to create a component, you have to go to here assemble and you have to create a new component. Inside every component, we have separate body and a separate sketch. Each and every component is independent of each other unless and until they are a sub assembly. That means if you're creating assembly by clicking over here and making a new component, it will make a sub assembly over here. You have to pay attention that whenever you're creating an individual component, you need to switch this one on. This is your main head assembly. From there, you can create a new component. Now, what's the difference between a body and a component that has to be understood? For that, let's start a new design. Let's create a simple body, a simple box. As soon as I do that, a body is appearing in the browser itself. We can copy it and we can paste it. It's like two bodies over here. Next, let's click here in the head assembly and create a new component This time also let's create a box in the same plane. Let's select this and copy. Then in order to copy also, you have to select this one, press copy, paste. These two bodies are actual bodies and these two entities are components. Now what's the basic difference? These bodies can be a component, but a component cannot be a part of a body. Basically, what happens when we are making assembly, we cannot utilize these bodies. When I click on joint, which is the most basic thing for assembly, the bodies get hidden, but the components are there. You can provide joints between two components. They can be joined, but the same thing is not possible with bodies. That's the basic difference. One more thing from these bodies, you can write, Click, and you can create them as components as well. But it is highly recommended that you always create a component from this assembly or this assembled tool bar by clicking over here in the head assembly. In the next lecture, we will start with a very simple assembly. We will understand how to create joints, how to create components. Then we will propagate to something complex like this Geneva mechanism. 6. 06 How to create joints: Now that we know what are bodies, what are components, and what is the top down design approach of fusion 360. Now is the time to understand how to create joints. The assembly making process of fusion 360 will be explained very comprehensively in the coming lectures. But the very first thing that you need to learn is to create joints. Now for that, we are having these four components over here. Now the very first step in any assembly making process is to ground any one of these components. To ground any component, you have to just right click, you have to ground it. The reason behind the same is with this grounded component, we can have a relative positioning for all the joint making process. Now, there are two types of joints in Fusion 361 is a simpler joint. The shortcut for the same is J in the keyboard, and another one is as Bill joint. The shortcut for the same is Shift plus J. Let's understand the simpler joint first. For this, we can go to this joint over here if it is there in your case, in your software. Or you can simply go to assemble and go to Join, or just use the keyboard shortcut. As soon as we click here, you will see the grounded component is having a wire frame like structure, and all the other components are highlighted. As soon as I howard the mouse over any of the component, you will see a icon is being made. This particular icon is what we call a joint origin. This joint origin specifies that this particular part of the component will go to another component. Let's select this particular point, this face of this particular component. You can also select this edge and it will automatically trace to the center. Let's select this. Now, with logical reasoning, you can tell that this will go inside of this. If I'm selecting this edge, it's not the inside, it's actually the outside of the hole. We have to be very vigilant for providing the joint origin. This is the second joint origin we are going to use for one particular joint. For this, let's select this and you will see that the first component will automatically track to here. As soon as the position is defined, you can provide the motion now. Now in this we are having lots of options, lots of joints, basically. First is the rigid one. You can animate or you can preview the joint motion from here. Second is revolute. Here, you can rotate the joint in any axis. Let's say it's X or Y or jet. You can make it custom and you can select any of the surface. Let's deselect and select another one. The joint will behave as per the selection of the surface, let it be gadexisly. Then we have slider, cylindrical pin, slot, planar and ball. For this particular joint, we are good with revolute only, let it be now here the rest revolute and slider joints will be explained in basic assembly section. Cylindrical pin slot and planar joints will be explained in intermediate assembly section. And lastly, the ball joint will be explaining advance assembly. We are going to have different practice exercises or multiple practice exercises for each and every joints in the coming lectures. Now as soon as you are satisfied with the position and motion of the joint, you can click on Okay. Then you can see this icon is being made over the joint. We will have different type of icons for different kind of joints that you will get to know gradually as you move on or progress in the course for revolute this flag like icon is being made. When we double click on this icon, we can change the orientation. Let's say I'm just rotating it by 180 degrees. Click on, Then if you want it to revert back to the original position, you can always click on Revert position. Or here it will be reverted back to the original position. But if you rotation that we have provided, let's provide a 90 degree rotation this time. Now if you want the rotation that you have provided or the new orientation that you have provided to be the default orientation moving forward. Then click on Enter and you can click on Capture Position. Now let's say I'm again making any changes, I'm reverting the position. It will revert back to the new capture position. This is the beauty of Vision 360. Moving forward, we need this particular pin to go inside this hole. Now for this, we can again invoke the joint command and we can provide the joint origin as the center of this pin for providing joint origin to this base component which is a grounded one. We are not finding any prominent point to snap or basically a prominent point to provide the second joint origin for the joint. For what we can do, we can select this inside area of the hole. You can see the center of this particular component is highlighted where we can fit the pin. But we cannot go over there just by howering the mouse. What we can do, we can select the inner portion, just by howering the mouse over there. And you can press and hold control or command in case of Mac users. And then you can just howard the mouse to that point and left click, let the motion be rigid only and click on. Okay, this was all about the simpler joint. Now is the time to create a As built joint. Now for as build joint, you need to have one component made over another component and it is already fixated at a point. That means position is already defined. You have to provide motion only. In these two cases, position was not defined, this sin was outside this component, this number one component was also outside. And then we have provided the position. But in case of aspljoint, position has to be defined earlier. That means, let's say we have created this second component over this first component for Aspljoint. Go to Assemble, click on Apljoint, or you can use the keyboard shortcut ship plus J. Then you have to simply select the component anywhere. Let's select this component and then select this component. Then you have to provide the joint type. It can be site revolute cylindrical slider, all the joint types will be available, just like the simpler joint. And then you have to snap to one particular point. Let's snap to this point inside. It will also have the same effect or the same outcome as the simpler joint. But in my opinion, using this joint simpler joint is more effective because with as Bill joint we are not providing any position. We are just providing motion. It takes away the essence of assembly making process. That's why I have used lesser build joints. In this course itself, I have used the simpler joint only because this is more down to earth and practical approach of assembly making. But you don't have to worry. I have covered a lecture dedicated to build joint with a men follower mechanism. You can also replicate all the assemblies that I'm making with build joint if you're comfortable with it. Thank you so much. 7. 07 A very simple assembly: Now let's understand how assembly works in Fusion 360 by making this very simple assembly. As you can see here, it's a circular plate having a pin attached in the center and a pin attached here with the handle. The objective here is to rotate this circular plate when we drag this handle, whenever we are making any assembly, you need to define the objective, how the assembly should work. This should be your primary focus. Prior to making the assembly here, we have to rotate the circular plate by dragging this handle. This is the primary focus here. What we will do, we will recreate this assembly when we are recreating this. When we are creating anything in this assembly section, we are not using proper dimensions. It's not two dimensions. Let's create a new design. Now here we have three components. One is the circular plate with a pin over here somewhere and a circular hole in between. To make it more comprehensible, let's hide the other two components. This is component number one. Let's make it first go to Assemble New component. Click, Okay. As you can see, a new component is added to the browser. Create a sketch. Select a vertical plane, circle command. Make any dimension because it's not two dimension. Make a circular hole over here and drag this area for pin. Finish the sketch. Let's press, pull it backwards. Let's make it minus five. Switch on the sketch. This, we forgot to press, pull this one. Okay, let's make it two side so that we can press from here as well. For providing the handle, our first component is ready. Let's hide the sketch. Double click here and write it as a circular plate. Now for the next component, let's push them on. For the next component, we need to have a pin over here in the center of the circular plate. What we will do, we will again invoke the head assembly. We are not invoking it. If we are having this component activate and we are creating a new component, then it will become a subcomponent of this component, which is not desirable. For now, let's activate this one and create a new component this time. Select this phase, this is very much visible. Create a sketch, make a circle from this end, select it, Press pool, let it be two sides. So that we can cross over here to somewhat like this. The most important part is this operation would be obviously a new body and a new component has been created. Switch on the head assembly and you can see, let's name it Pin. Now for the last part, we need to create this handle over there. This would be the last component for that. Again, just check if this is activate or not. Go to assemble tool bar, create, new component. Create. Okay, select this face of the pin that we have extruded from the circular plate. Create a sketch. Let's create a circle. The fit point is fine. Invoke the line command. We're almost done. Just stream the unwanted areas just for consistency. Make them and finish the sketch. Now select this reason that we have created right now, press pull it backwards. I think this much would be sufficient. Operation is obviously new body click. Okay, Now this is a handle. You need to provide specific names for each and every component because what will happen if you're having like ten to 20 components in your assembly? You will not be able to understand which component is which one. That's you have to make a habit of providing Nomcalsa, providing name to them. Now, everything has been prepared. All the three components, they are individual and when we drag them, they can be go out like this. Now, if you accidentally did this, you want to revert it to the original position, Just click here In the revert, it will be reverted back. Now comes the fun part. Now we are going to provide joints to them. Now, joints are that lets components to have relative motion between each other. For that, we can go to assemble and joint, or you can use the shortcut key Jin, the keyboard. Just click here, this one again, and make the motion revolute. Click. Okay. Now as you can see, the motion has been provided. But these two components are attached together, but they are moving here and there. What we need in such kind of situation is that we have to ground something. Let's ground this one. Now we can have a relative motion between the circular plate and the pin that is in the center. But as you can see, this grip, this handle, is not attached to this one. This spin, we have to do that. Let's revert the position again. Click J, start the joint, select this one, select this one, and make the motion as rigid. Click Okay. Now as you can see, we have the desired rotation or basically our primary focus has been attained with this very simple demonstrative assembly. I hope you got the idea of the steps involved in the assembly making process of future 360. By considering this lecture as a milestone, we can propagate further to create basic assemblies like Universal Joint Garden, Joint knuckle joint and Geneva will mechanism. Then we will propagate further to create some intermediate assemblies with some intermediate joints like cylindrical planner and pin slot. Finally, in the advanced assembly, we will understand about some advanced techniques in the assembly making process of fusion 360. 8. 08 Universal Joint: Now, the very first assembly that we are going to create is of universal joint. A universal joint is a joint, or coupling connecting rigid rods whose axes are inclined to each other. And is commonly used in shafts that transmit rotary motion. It consists of pair of hinges that we call. They are oriented at 90 degrees to each other and they're connected by a cross shaft that we are calling center block. Here, I have made this assembly beforehand for reference in order to have a better understanding of how each and every components are connected to each other. Now let's start with the assembly. Just click on New Design. Let's save it Control. Let's name it Universal Joint Exercise. As you can see in the browser itself, the untitled status is changed to the name of the file itself. We are calling us a head assembly. This one is the head assembly. Now the first component that we are going to create is this. F. I have hidden all the other components because we are going to create each and every component one by one. First we're going to create this particular component, the folk. For this, go to assemble Toolbar. Always go to Assemble Toolbar when you're trying to create a new component. Let's name it Folk, invoke rectangle command. The keyboard shortcut is R and select any of the vertical plane. Let's select this one. As you can see, as soon as we have invoked the rectangle command, we're having a sketch palette over here in which we are having option to change the type of rectangle we are going to make. Let's select center rectangle from here, then provide any dimension because all the assemblies that we are going to create in this course are not two dimension because my aim is to make you familiarize with the assembly making process in Fusion 360. You can incorporate dimensions as per as your requirement or as per as your client's requirements. I will let you know wever some crucial dimensions are required as per move forward in the course. Let's select any dimension. For now, click on Finish the sketch, select the cason, press pull, then select this particular phase. Invoke the circle command by pressing C in the keyboard and create a concentric circle. Again, let it be of any dimension. Press pull this one outwards and click on. Okay, we're done with this particular section of this particular component. Now we will be creating this profile. For this, we will select this particular phase, invoke the circle command, trace the origin, make a bigger circle, then inside a smaller circle whose dimension we are going to remember. Let it be like 15, better make it 18. Invoke the line command by pressing L in the keyboard. Select this particular point and select a point in which tangency constrant is being made, as you can see here. Similarly here, if by mistake you have lost the tangency constraint, you can always get it from here. Select the line. Select the circ, let's trim some unwanted areas. Finish the sketch. Select the reason, press pull it downwards. Now as you can see, we need this particular profile in the bottom as well. What we will do, we will invoke the mirror command, select the feature, select a mirror plane, and click on this. Here creates our first component, that is folk. Now we have to create another component, focus number two, which is like 90 degrees inclined with folk number one. Now for this, in order to propagate to second component, we're going to make a slight adjustment here. We are going to use the inspect toolbar and component color cycling toggle the shortcut for the same ship plus N. When we click on here, the color of your component is changed. As soon as we create new components, its color will be also changed. Same thing is happening here as well, because it happens in all the files in Fusion 360. Now invoke the or, basically activate the head assembly. Left click and select this particular component. Control C, control V. Just drag it outwards, rotate it by 180 degrees and again rotated by 90 degrees. Our second folk is also created. Notice it is having the same color as the first component because it's a carbon copy of the first component. As soon as we create a new component, its color will be changed. That is the beauty of this particular tool component color cycling to now. Next what we need a center block for this. Again, just see if the head assembly is activated or not. And then go to assemble toolbar new component. Let's name it center block. Select this particular phase and invoke the circle command. The outer circle should touch the outer circle of the profile. The inner circle is obviously 18 millimeter that we have chosen. Select this profile, press pull it and make the extent type two object. And select this, obviously the operation would be new body for a new component. Click on Okay. As you can see, this new component is having a different coloration. This comes very handy when you're creating a very huge assembly and you need to maintain order with separate components. Now, activate this center block only here. We will create certain sketches. Create a sketch on this particular plane. Create a circle somewhere over here of any dimension. But the inside circle should be of eight millimeter. This we are doing because we are going to fit a pin in between this at the sketch. Let's hide these two folks as of now. Now just measure the distance of this one. This is 60 millimeter. What we will do, we'll select this profile. Right click, press pull. Let the direction be symmetric, the distance should be 60 divide by two. Operation should be joined. This created our center block. Or let's activate the head assembly again. Now what we are going to do, we are going to create this particular pin. Now for this, again, go to Assemble toolbar, new component. Let's name it Folk one pin. Click on, okay, select this particular surface. Invoke the circle command. Select the profile, and again make the extent type as to object. And select this particular surface. Click on. Okay, select this, Press pull, let it be like five MM up. And the same thing in the bottom as well. Five millimeter. Now here, let's create a circle, a bit larger diameter. Select this profile, right click, press pull again to object. An object would be this one. An operation is joined because it's part of this component, only the folk pin. Now next we are going to create this particular caller. For that what we will do, we'll again activate the main component. Main assembly, Head assembly. Go to new component. Let's name it. Caller, select this particular surface. Invoke the circle command, let it be of any dimension. Finish the sketch, press pull it, Trent type again to object operation would be obviously new body and click on. Okay. Now activate the head assembly again. This time select this particular phase and create a tangent plane. Now this plane, let's create a circular hole. Now in order to do that, we need a point to snap somewhere. What we will do, we will project this particular area clock. Just create a line from the midpoint of this to midpoint of this one. Let's convert it into a construction line. Now from the midpoint of this construction line, let's create a circle. And let's remember its dimension as well. It's three millimeter. Finish the sketch, select this right click, press pull and cut through All notice that we are cutting through one component and it is cutting through the second component as well. Because the head assembly is activated. Now almost all the components are made. Now the only thing that is remaining is to create identical components. This color and this pin. These two components, this color and this folk pin will go here as well. We have to create a copy of these two. Just control and select both of them. Control C control and just drag it outwards. It has created two new components. Now the last component would be a lock, that is, that has to go between these. For this, we will again go to assemble toolbar, new component. Let's name it Lock. Let's create a sketch on this plane, only somewhere. Let's say here. As you can remember, the dimension of lock should be three millimeter. Now we have to press, pull it outwards to create a three D model. Now how much to press pull that we have to inspect from here. That would be dimension of this color. It is like 26.8 double three millimeter, we will be excluding it. 26.8 double three. Click on. Okay. Now we need one more lock. We will again activate the head assembly. Left click on lock control C, control V, and one more lock is created. Now we are officially done with all the components. Let's drag them outwards. And see we have 22 colors, one center block, two pins for folk, and two lock pins. Now it's time to create the assembly. All the components are here. Now we have to provide joints. Now, in order to do that first, let's revert the position by clicking here. Now, in every assembly, we need to ground one particular component on the basis of which all the other joints, all the other components will be clubbed together. Here, we will be grounding the center block. That means all the other components are free to move as of now, but this center block will not move. Let's track all the components out and let's start providing joints for joint. Again, we have to go here or we can use the kibo shortcut J. Select this particular phase and select this particular phase. This joint should have motion of revolute. For the next one, again, click J on the keyboard, Select this particular phase and select this particular phase. You have to be very vigilant when you are creating the joints. You need to understand which particular phase or which particular portion of the component should go. Where. Here also the motion is revolute and click on. Okay, next is providing these pins. Just select this particular phase. And this particular phase, it should not be a revolute, it should be a rigid one. Click on. Okay, let's see if this is rotating. Yeah, it's rotating. Now, attach a color to this pin. Click on joint, select this particular edge, basically this particular edge, similarly here also. And then just attach these lock pins, select this particular edge and select this particular edge. Similarly here, also select this and select this. Now our assembly is fully complete, but as you can see, when we are rotating, it is overlapping with other component. Same thing is happening here as well. What we need is limits. We can provide limits to all these joints by going to browser and selecting the respective joints. Let's select this particular joint. Right click and addit joint limits. Let's select the right phase so that we can clearly see what is happening. Or better select the top phase. Now for universal joints, the ideal limit is between -32 to 30 degrees. We will be using that initially. Provide the rest position, that is at zero degree as of now. Then provide the minimum S -32 maximum 30. Just animate it and see Perfect. Click on Okay. Same thing we have to provide with this particular joint. Let's go to the right view. Rest is at zero, minimum -32 maximum 30 degrees, and click on, Okay, Hide the joint. And our assembly is officially complete. The color that you're seeing here is because of this component colored cycling togger. You can switch it off as soon as your assembly is completed and you will see this gray coloration in all the components. Then you can go to the render work space and provide the rendering of your choice, just like here. 9. 09 Knuckle Joint: The next assembly that we are going to create is of a knuckle joint. A knuckle joint is a form of pin joint that's used to transmit tension loads while allowing rotation in one of the plane. There are many applications of this particular joint, like link of roller chain, bicycle chain chain types of watches, connecting rods between locomotive wheels. All mechanism of a reciprocating engine, Windchill wipers of a car, and the list goes on and on. In this assembly, we are having four major components, the Eye and Ok and knuckle pin and color. One minor component that is taper pin. Here also, we will follow the same procedure of concentrating on one component at a time. First, we are going to make this component, let's hide all the other ones. Now in this component, we are having one particular profile perpendicular to another. Let's create this one by creating a new design. Go to assemble toolbar and create a new component. Let's name it. I end now. Create a sketch in any of the vertical planes. Let's create a circle by invoking the circle command. The shortcut for the same is seen in the keyboard. Let it be of any dimension. Let's press pull it outwards. Now here as you can see, this particular profile is perpendicular to this particular profile, and it is joined by a rectangular extrusion. So what we will do, we will create a sketch, a face sketch in this particular plane, which is perpendicular to this particular sketch, or basically this particular profile. Let's create a concentric circle. Let's trace the origin. Let's place it somewhere here. Now for the inner circle, you have to remember the dimension. Let it be like 25 men. Finish the sketch, select the profile that is generated. Press pull, Direction should be symmetric. Let's extrude it outwards. I think this much is sufficient and click on. Okay, now we are having this rectangular extrusion from this particular profile to this particular profile. What we will do, we will select this and create a sketch over this one. But as you can see, this second body is hindering our sketch. What we will do will go to the end component and we will hide the second body. This is the first body. This is the second body. We are going to hide this one. Now we can create a sketch over this. Let's create a rectangle. A center rectangle, to be precise. Let's create a square like structure. Finish the sketch and show second body as well. Now select this vision, right click, press, pull, make the extent type to object and select this surface. And click on Okay, the Outline of Folk and is completed. Just one detail is required, that is this particular section of the model. For this, we will select this particular phase. Invoke the line command by pressing all in the keyboard. Select this end. Select any point over here. Select any point, a vertical one. Then press and hold left mouse button so that we can create arc and just close the region. Now finish the sketch. Select this region and invoke the revolve command for the axis. Select this and click on this. Particular profile has been generated, but this is required in all the four corners of the rectangular extrusion. What we will do well. Creator circular pattern. Then select the feature. Here we are having types of faces, bodies, features and components. Here we will be selecting feature because this is a feature that we have generated here. Then for the axis, we have to select the green axis over here, which is not visible as of. Now what we will do, we will zoom out. It will be visible. It, yeah, it's good to go. Click on. Okay, our first component, the eye end has been created. Now let's move on to the second component, the fend. This foc end is like dependent on the ion itself. We'll be using this as the reference. But to create any component, you have to activate the head assembly. Then you have to go to Assemble, Cuba and new component. This time Writers and click on. Okay. Now select this particular surface and create center rectangle. Let it be of any dimension, but you have to make sure that it is larger than the outer circle diameter. Let's finish the sketch. Select this profile. Let's select this one also, right click, press pull, Make the extend types two object. And select this surface. Click on okay. Then select this, let's say let's extend it by ten MM. Here, let's extend this one also by ten M. Now what we require is this fork looking structure we have created up to this much only except for the hole that we will be creating next. For this, what we will do, we'll simply select this particular phase. Let's start creating a sketch now. We don't know where this component is inside of this particular extrill. Will go to project and select this particular body completely. Click on okay, the body has been projected to the sketch itself. Now we are having a clear idea from where to make the cut. Now invoke rectangle command again. This time two point rectangle. And select this point by tracing from the projected sketch. Finish the sketch. Select all these profiles by pressing control, right click, press pull all the way down. But as you can see, this is also cutting our previous end component, which is not desirable. What we will do in this extrude pet, we are having objects to cut here. De select the end and click on. Okay. Now again, select this phase, Invoke the line command, Select this particular end, hold this left mouse button, and select other end. Similarly from here, hold the left mouse button and select this hand. Notice the region is not closed, so we have to close the region as well and then finish the sketch. Now select this profile, press pull again, extend type two object, and select this particular phase. Then is almost created except for a hole over here and this particular profile. Now we will create a hole in this particular phase. Again, project this body. Clickon, Okay, invoke the circle command and create a circle of 25 MM. Select this, press pull, let's create a hole. Now for this particular profile, we need to create a plane over here. Let's create a tangent plane. Let's start sketching on this one. Now here we need to find the center point of this particular profile. For this, we will again use the project include command. This time in the selection features, select a specified entity, all these four edges. Now invoke line command, find the center of this one and center of this one. The midpoint is denoted by this triangular icon. Now let's create this as a construction line because this is not a part of this particular assembly. Then create a circle in the midpoint of this construction line. Let it be again of any dimension. Finish the sketch. Select this circular profile, press pull outwards. And select this phase, create one more circle, a bit smaller, one. Finish the sketch, select this one, press pull outwards. Now, in this particular phase, let's create a rectangle. Let's trace the origin. Select the whole region of the rectangle that has been created. And press pull it like this. Now we need like four of the insertions. What we will do, we will invoke the circular pattern, Select the feature, this one. And select the axis. Now again, the axis would be this green one number of object would be obviously four and click on. Okay, and is also created. Next, we need a pin in between a knuckle pin. For this, we will again activate the head assembly. Go to Assemble Toolbar, New Component. Let's name it, knuckle, Spin, and select this phase. Invoke the circle command and create a 25 MM circle. Select this, press ext type two object, and select this. Click on, okay, select this phase, press pull, let it be like ten MM outwards. And same thing in the other side. Next we will create a color. The next component for this, select the extruded pin over here, and invoke the cycle command. You select this region again to object and select this, and click on, okay, obviously the operation would be new body. Now activate the head assembly, and this time select the color component and construct a tangent plane. Now on this plane, let's create a circle of let's say four MM. Finish the sketch, select the profile press, pull it, and let's create a hole through both the components, that is the pin and the color. As you can see. Now the last thing that is required is a paper for this. We know this one. This particular hole is of four MM of diameter. Now we have to see what is the diameter of the color. It's like 37.5 do seven millimeter. You can always check anything from this inspect tool bar, the measure tool. Basically the shortcut for the same is in the keyboard. Now create a new component. Let's name it taper. Create the sketch on this plane. Let's say invoke the circle command. Yeah, it was four. Mm, finish the sketch, select this one, pull it like 37 somewhat, but provide it a bit of taper. Let it be like minus three degrees, it would be very less, let it be two, or let it be one only. Now, all the components of knuckle joint has been created. The end, we have the fork, we have a knuckle pin color and a taper pin. You can always revert to the original position by clicking here, But as of now, let's move them out here and there. Now in assembly, as I told earlier, we need to ground at least one component in order to have a relative motion or relative movement between other components. We are going to ground the and click on Capture position. Now the first joint that we are going to create is between the I and the foc end. Just click here or go to Assemble and click here. Or you can use the shortcut key J in the keyboard. Select this particular end and select this particular end. The motion would be obviously a revolute one click on. Okay. Next we have a pin that has to be inserted between the hole over here. For this click on joint ended, the motion would be Sid. But here we have to get this particular pin outwards, like ten MM outwards because this much that we have extruded earlier. Now next we have to provide color. Go to joint, select this face, and select this phase, and click on, Okay. Lastly we have to attach this taper pin for this. Again, go to joint, select this end, select this end. As you can see, it is protruding outwards, which is not desirable. So what we can do, we can flip this component over the joint origin. This is flipping over the joint origin and click. Okay. Now our knuckle joint is complete, but as you can see, when we rotate this joint, it's rotating like 360 degrees. It is overlapping with the fo can component which is not desirable. What we will do, we will go to joints, select the revolute that we have provided, right click and added joint limits. In this case, let's make zero degree as the rest. For minimum we'll provide -32 or basically -30 degrees. For maximum, let's provide 30 degrees. Just animate it and see. Yeah, it looks good. And click on Ok. Finally, our knuckle joint is officially completed. 10. 10 Carden Joint: Now next we are going to create this Cardon joint, which is like a modification of universal joint. Now for this we have certain components. We will be starting with this yoke one. Let's hide all the other components. Let's focus on this yoke component. Let's create a new component named yoke. Now we need to create this sketch profile for this, Let's start with a rectangle. A center rectangle, to be precise. Start from the origin, let it be of any dimension. Then click on the keyboard to invoke the upset command. Select this rectangle, upset it inwards. Click Enter. Invoke the line command. Select this point, select the outer rectangle, same thing here, and presenter. Now let's trim these two lines. Let's get rid of these construction lines as well, and finish the sketch. Now, select this region, press Pull, let it be asymmetric, Let it be five MM only. Again, dimensions are not the concern. You can provide any dimension of your liking. Or if you are having any specific dimensions, you can provide it here. Now, we need this particular profile for the select this phase, Create a concentric circle, basically a pair of circles we are creating and finish the sketch. Select this region in between, right click, press pull, and creator cut. Now as you can see, the sketch is gone. So we can again show it by clicking in the browser, in the corresponding component, and in the sketch, this is sketch number two. Select it. Now select all the outer regions. Right click, press pull. Then select any of the surface, and let the operation be joined. Click on, okay. Now hide the sketch. As of now, this particular profile has been created. Now we need this profile in the top as well as bottom of the yoke. For this, we are not going to create any sketch. We are going to invoke the primate entity, a cylinder. Just select the surface, you can see the origin is visible over here. Just trace it, unless you're getting a midpoint symbol, as you can see here in this particular edge. Then create a cylinder on this time. Select this surface and make the operation Us Join. Click on okay again, right click Repeat Cylinder. Select this face and find the center point of the previously created cylinder and create another cylinder. Now we need this profile in the bottom as well. What we will do, we will invoke the mirror command for the type we are selecting feature. For this, you can simply left click in the time line. This one also select the mirror plane and it is created. Our first component is ready If we switch on the complete assembly, the pre made assembly over here, you can see this component has a identical twin. What we will do, we will invoke the head assembly. Let's save it so that the head assembly can have a name. Let's name it card. Now here as you can see, the head assembly is activated. We can left click on the component, Just control C and control. And if we can paste another component, identical twin, let's drag it outwards just to a sufficient distance. Now both of our are created. Now we need the center blocks. Let's hide other components and just see how the center block is looking. Create a new component. Let's name it center block again. Invoke cylinder command, Just hower the mouse by selecting surface. Just hower the mouse and find the center point. And create the cylinder up to this particular distance. And click on. Okay. Now in the center block, we need this cut by creating a sketch. We can do it easily, but there is another way as well what we can do. We can invoke the head assembly. Click on combined from the modified toolbar, Select this component, select this component, and let the operation be cut. And do not forget to keep the tools. Now when we drag this outward, you can see this profile is generated, just revert the position. Now as you can see this complete assembly, you will notice that the center block also has a identical twin. What we will do, we will again left click in the center block. Just copy paste, Let's drag it outwards to a sufficient distance. Now in the center block, we are having a hole for fitting this spin. What we can do, we can select the surface and construct a tangent plane. Click on okay, select the plane great circle. As you can notice that we cannot find a center point anywhere we can project this body. Now from the midpoint of the top edge and the midpoint of this bottom match of the projected sketch, let's create a line. Let's make it construction. Now, from the midpoint of this newly constructed construction line, we can create a hole, let it be a 15 MM. This dimension may differ in your case, because it depends upon how much larger you are making your. Or you can have a specific dimensions depending upon your necessity. Let's finish the sketch like this. But the idea over here is to remember this dimension whatsoever, dimension you're taking to create this hole. You need to remember that dimension because we are going to create a pin based on that dimension, as I told earlier in the very beginning of the course. Also that you have to take care of certain dimensions, those are interrelated with certain other components. These dimensions are provided by you only. It's not like there is some sketch on the basis of which we are making the assembly. There is no such sketches, there is no such drawings. We are just making the assemblies out of the air. If you are having dimensions, you can make it easily. But the idea behind this course is to make you familiarize with the assembly making process. In my opinion, you should not be dependent upon dimensions earlier. Because if you get the flow of making assemblies, you will easily make any assembly without the need of any dimensions. But in standardized point of view, dimensions are necessary. They are very much required. But before adding dimensions to the assembly, you must know how to assemble. You must get the feel of making assemblies. That's the basic idea behind the course. Getting back to this one, we have created the center block, both of them. Now we need a pin for that. Let's create a new component. Let's name it pin. Let's create a circle on this particular plane anywhere. But here, dimension would be 15. It can be different in your case. Finish the sketch, select this region, press pool, make it symmetric, and just drag it outwards. And click okay. Now on this face, create a circle of any dimension. Select this, press pull inwards, and click on, Okay. Now create a mirror, select this feature, select the mirror plane as this one. And click on Ok. Now, as you can see in this premade assembly, we need this particular profile somewhere over here as well. They both are like joining, it's a single component, but having multiple bodies. What we can do, We can go to this pin component, we can go to the body and we can control and paste another body. Let's have a sufficient distance. Click on Okay. Now on this body as create a two point rectangle. As you can see, the center of this one is highlighted, but center of this one is not what we can do. Again, project, press in the keyboard. Let's select this Sketch Entity and click on Ok. Now, when we invoke the rectangle command, you can see, or even in fact any command you can see. The circle, center of the circle here. From this center to this center. Let's create a two point rectangular and finish the sketch. Now, from this profile, this sion, just press, pull it up to this particular surface. Obviously the operation would be joined only click on. Okay, Now we need the same thing in the other side. Just select this feature, select the mirror plane as this one, and click on. Okay. Now as you can notice, this is a single component. That's why we have copied and pisted this particular body over here. Now almost all the components are ready. Just these two shafts are required for this. What we can do, we can go to assemble again new component. Let's name it shaft. Create a cylinder from this surface. This is the center, just extrude it outwards. I think this much is sufficient. Click on, okay. Now invoke the head assembly, Select this shaft. Just paste it and move it to sufficient distance. And click on, okay. Now all the components are created. Now the only thing that is left is to create the assembly for this. Let's ground something. Let's ground the shaft. Let's drag all the components here and there. Let's start providing joints. The first joint that we are going to provide is between yoke number one and the shaft. The motion is obviously revolute about jet axis. You can change the revolution just to see how it does, but initially the revolution, the axis of rotation is perfect. Click on. Okay. Now for the next joint, select the center block. This is small detail that we have created. The small cut, this part of the yoke. Again, the motion would be revolut only about dex. Next right click, repeat the joint. You can also use short cut J in the keyboard. Select this particular point, you need to select this middle point over the center block. For that you have to press on control and just drag the mouse over there. The joint is created. Now we need to attach a center block here as well. For this, again, joint control. And select the center of this one and center of this one perfect. Now as for this yoke and this center block, let's select this bottom one and select here. Okay, just double click on the joint that we have created. The revolute one and just revolve it by 180 degrees. Perfect and capture the position. By capturing the position, what we are doing, we are basically telling the software that we want this configuration. As of now we can. Let's say I'm rotating this shaft here and there, and I'm capturing the position again. I'm moving the shaft anywhere, or moving anything anywhere. When I am clicking on Revert position, it will be reverted to the captured position. This is the beauty of Fusion 360. Now the last joint would be between this shaft and this yoke. This would be also revolute. Now, before finalizing this assembly, we need a slight modification. Just press M in the keyboard to move this pin. Let's move it by 22.5 degrees. This is the standard for a cardon joint. Again, use move command select the yoke, this. Ok? Let's move it, okay, this one and move it also by 22.5 degrees. This is the standard orientation for any cardon joint. That's why we have done this. Finally, let's ground shaft number two as well and capture the portion. Let's hide the joints. Just animate the model by selecting any of the joints perfect. So our carbon joint is also complete. 11. 12 Geneva Wheel Mechanism: Now as promised, let's create this Geneva Mechanism from scratch. Now, what is this Geneva Mechanism? Geneva Mechanism is the most commonly used mechanism for producing intermittent rotary motion. It is characterized by alternate period of motion and rest with no reversal in direction. It is also used for indexing, like rotating a shaft through a prescribed angle. Other applications of Geneva Drive includes automatic sampling devices, banknote counting machines, indexable equipments like tool changers in CNC machines, and many more. Let's create this particular assembly. Now here, as you can see in the browser itself, we are having four different components. First is the follower, which is a driven component. Then we have a Cam, which is driving the whole assembly. It's a driving component, a pin, which is attached to the follower and which is attached to the can. Basically, we can say we have two basic components, follower and Can. We will start with the follower. For that, let's create a new design. As I told earlier, always start with a new component from the assemble toolbar. Let's give the name Follower. Now here let's hide all the other components. The follower be visible as you can see here, this component is clearly having circle as the measure sketch entity out of the circle. All the shapes have been carved out and the component, the follower is made. What we will do will create a sketch on the horizontal plane. Invoke the circle command. This assembly is not two dimensional. You don't have to worry about providing dimensions here and there. Just go with the flow. Let's create a line. Let's pray the origin from here. Let's make it coincide with the origin itself. Let's make another line over here. Let's say at angle of 54 degrees. Invoke the mirror command. Select this line. Select the mirror line. Click. Okay, let's convert these to us construction line. Let's get another circle somewhere over here and make it tangent to this and this one. Let's convert this to construction as well. Now again, make a circle from the center point of the construction circle that we have created and give any dimension. Now create a slot center to center slot on this line till this in section point, let it be of any width. Now what we are planning to do here, we are trying to recreate this particular section of the component, this one. That's why a slot has been created. Now create a circular pattern. Double click on the slot to select all the four objects of the slot. Select the center point, give quantities of five, y five, because we are having five symmetrical, or basically similar sections in this component. Now what we will do, we will try to recreate this particular section of the component. Now for that, let's trim, let's remove this one, also better create it as a construction line only. Again, invoke the circular pattern. This time, select this particular arc, select the centerpoint, and provide five first the quantity. Now all that is left to create this component is to trim the unwanted areas. We are going to fast forward this particular section. Since everything is trimmed, finish the sketch and take the reference from this premed assembly of how much we have to extrude. We have to extrude to five millimeter. We're taking reference of how much press pull command we have to use, up to how much we have to extrude a two D sketch to a three D model. That's the only reference we are taking with this premed model. Let's select this one, Press pull five millimeter upwards. Our first component, the follower is completed. Now for the next one that is the can activate the head assembly, new component. Let's name it Can. Now for this, what we will do, we will make the sketch of the previous component visible. Let's create a sketch on this plane itself, from the previous component. If you can see the circle, the construction circle, we can project it. This we have discussed earlier in one of the sketches. This one, click on, okay. It's been projected to the sketch that we are creating right now. Now, again, create a circle from here. Try to make it coincide with the arc. Or here, make one more circle and a small circle over here. Right now what we are trying to do, let's hide the follower for now. We're trying to recreate this particular component, the Cam one. For that we are creating this profile. Let's create one more circle over here, just trace the origin. This circle corresponds to this particular pin which is made on the Cam itself. And what this pin is going to do, as you can see, this is having contact with the follower and it is rotating it. This is important in this assembly. It should not be more than this gap. Let's check the gap once between these two points. It's 6.221 We cannot make it more than this one. Invoke the circle command. Just stress the origin. Let's make it five, only now we have to create this particular section of the cam. For that, what we can do, we can create a line anywhere from, let's say here, trace the origin, this one. Let's make it tangent to the circle. This one also. Then let's make it original vertical. Click on modify, provide, fill it. I think this much will be sufficient. Present we are almost set for the cam, but here we have to generate this particular profile for that. What we need is a three point arc. Let's say somewhere over here to here. Just stream the unwanted areas. We're almost good to go. Just finish the sketch. Select all this, I just switch out the follower for now. Right click and we are to extrude it downwards. By how much? Let's check it from here. Three millimeter. Remember, you have to provide a space for the pin of the can, that's why this is blank. Right click. Pull it down by minus three. As you can see, sketch is gone. Let's make it visible again. Now, again, select this one. Select this one. Also, extrude it upwards. Okay. We have to take the dimension here. Right now, what we're creating, we're creating this profile, this theory profile and this. Let's, let's measure it. It's like ten millimeter above. Let's select this right click, press, pull ten millimeter. Let's hide the sketch. And switch on the follower. Go to head assembly, and you can see two components are made. Let's hide the sketches for now. These two components are independent of each other as of now. But we will provide joints and we will provide attachment to them. Now, in any case, even if you are dragging the component here and there and they are in very different positions, you can always revert them back. Now the only thing that is remaining is the pin for the follower and the pin for Cam itself. For the follower, we need to create a hole over this one, let it be of any dimension. Right click, press pull downwards. Now we will create a fresh component to give a pin to the follower. Let's name it pin for follower. Select this face circle, select this one. Press pull it downwards to let's say 25 millimeter. Obviously the operation would be a new body. Click on. Okay, again, activate the head assembly. We are having now three components. Now the only thing that is remaining is the pin for the can. For that, again, let's create a new component, Rename it Pin can, click on Ok. Select this phase circle command. Press pull downwards and up to where let's make the extent type two object. And select this one. The pain of the follower, it will be extruded to that particular distance. Switch on the head assembly. Now we are having all the components in place. Now comes the time for visualization to understand how each and every component is interacting in the assembly. For that, let's go to this one, this premed assembly, as you can see. This is driving the follower. But these two pins are fixed. They are not moving. This follower is rotating on the pin of the follower. This cam is rotating on the pin of the cam. We are having a relative motion between them as I told earlier. Also, we need to ground certain things. When you try to understand this particular mechanism, you will come to know that these two pins, they are both grounded. They are both fixed. What we will do, we will right click on the pin of the follower. We will ground it, right click on the pin of the cam. We grounded. Now these two are grounded. That means I can freely move these two. The follower in the cam, but I cannot move these two. Let's reverse the position now. The follower and the pin of the follower, they are having a revolute motion. Similarly, the Cam at the pin of the cam, they are also having a revolute motion. Altogether, the assembly is having a relative revolute motion. What we will do, we will go to joint. The short cut of the same is J, the keyboard. Select this face and select this point for the pin, and give the motion as revolute. Similarly for the Cam, again, motion is revolute only. Now, as you can see, the pin that is supposed to revolve, the follower is like protruding out of the follower. This is not desirable, so what we will do, we will adjust it somehow so that it's not touching it. Let's check if any overlapping is there apart from this pin. I think there is none. Just adjust the pin in between over here. Now you have to capture the position. That means if I am rotating it anywhere, when we revert it back, it will revert to the captured position that we have did right now. I think we are good to go. Now provide context to all the surfaces and our assembly is complete. Now let's animate the model in order to see if any mistake is there in the assembly. Just go to joints, select any of the joint, and animate the model. As you can see, there might be chances that some overlapping of surfaces is taking place. What we will do, we will press pull this just a little bit, just like over here. And now animate the model. And our assembly is officially completed. Let's hide the joints. Let's provide rendering to it. And our Geneva mechanism is fully complete. Thank you so much. 12. 13 4 Bar Linkage Mechanism: Next we are going to create this four bar linkage assembly. It is the simplest movable closed chain linkage. It consists of four bodies that are called bar or links, connected in loop by four joints. It is used in many different devices like locking players, bicycles, oil well pumps, loaders, internal combustion engines, compressors and pentographsow. Here these bar or links have separate names as well designated names. This small linkage that you're seeing here, it is called the Input link. The bigger link that you are seeing here or the bar that you're seeing here, this one is called Output link. The one which is grounded or fixed is the fixed frame. The one which is joining the input and output link is called coupler. Rest Four components are simply pins that are provided in order to create revolution in order to create the assembly. Let's create this one. Let's create a new design, a new component. Let's name it Fixed Frame. Now here we are going to apply a different approach because the bar and links are dimensionally dependent upon each other. We are going to use dimensions in this particular assembly for this fixed frame component. Let's create a sketch on any of the vertical plane and just create center to center slot. Let the distance, the length of this slot be 100 MM and the thickness ten MM. Click Enter now finish the sketch. Press pull it, let it be this side only minus two. We are assuming anything. You can make it more thicker if you want. Now let's provide name for this assembly. Let's name it two bar only so that we can have our head assembly, a name. Now invoke the head assembly and create a new component. Let's name it Input Link. Now for this, select this particular phase of the previously created component, the fixed frame, and create a sketch. Again, invoke the center to center slot. Select this, select a distance, a length which is half of this one. We are going to write 50 here, center and for thickness, we are making it uniform. Tanamm need the sketch. Select the profile control. Press control. And select this profile. Also, right click, press pull this side. We are making thickness constant as well, so two MM can click on. Okay. Again, invoke the head assembly. This time also select the fixed frame. The surface of fixed frame on create a component, let's name it Output link here also escalator slot center center one. Again, the distance here, this is the longest link in the assembly Distance here should be more than this one. Let's make it a 20, let it be 110, only thickness is ten. Finish the sketch. Select the profile control, and select this profile as well. Press pool again, two MM. Again, activate the head assembly. The only thing that is left is a coupler which is joining the input link and the output link create a new component. Let's name it coupler. You can select this face of input link, or you can select this space of output link and create a sketch center center slot from the center of this one to the center of this one. Notice this is not snapping exactly to the center of what we need. Our favorite project. Command prep in the keyboard. Select the select. This we're selecting the sketch entities, not the body here. And click on, okay, we can find the center point. Now again, go to slot center, center, slot. Select the center point of the output link and the center point of input link. Again, width of the slot is ten. There is the sketch. This try to select multiple profiles, right click, press, pull again, two MM. Now our basic components have been created. Now the only thing that is remaining is to create these pin like components, four of them. Basically, because there are four links for that, we have to manually create holes in all the intersection of the links. Let's create here. First, let it be five MM. Finish the sketch, select this, just press pull and cut through. Now I'm going to fast forward in order to create all the other holes. Since all the holes are created, let's create corresponding pins for providing appropriate joints. Now we need four pins to put in these holes and then we can provide joints, just like over here. For this, just check if the main assembly, or the head assembly is activated or not, Then create a new component. Let's name it Pin. Now from this phase of the input link, let's create a circle of diameter five MM, because this is the diameter of the hole that we have created. Select this region, press pull up to the fixed frame. Basically, we are covering the hole completely. Now this particular component is similar to all the other holes. This pin, what we will do, we will activate the head assembly. Left click on the pin control C control, and just drag it outwards. Like this press. Okay, this will automatically snap to this particular hole, but the same would not be the case for these two holes. For this it can be. If we copy this one, the spin one only and paste it, we can actually move it to this point. Yes, it's almost snapping. When we are providing the joints, it will snap perfectly. Now let's select pin number two, control C, control V. Let's pull it upwards. Basically all the components are created just like this one. This is small details as you can see here that will be added afterwards. The assembly is fully complete, don't worry about that. We will add them also. Now we need to ground something as the name suggests for this particular component, fixed frame, we can ground this. Now let's remove the pins. Just the pins. Let's start the assembly for this. Click on joint select this particular phase of the pin. And this phase of the short link motion would be obviously revolute click. Okay, now here you might wonder that providing just one revolute joint to the pin and the linkage, we'll complete the assembly. But that's not the case because this joint is provided with respect to the shot or basically the input link. But for the fixed frame there is no corresponding links for this, what we will do, we will again invoke the joint command, select the other end of the pin, and we will select the fixed frame. Again, the motion is revolved only. Let's repeat the same process for all the other links. Now, since all the joints, corresponding joints are created, our assembly is complete, announced the time to provide these details. For this, what we will do, we will first hide the joints and we will make the head assembly activated. Now select the larger or the output link. Let's create a two point rectangle. Let's chum in and select some prominent point. Just drag it downwards. Select this press, pull, this one is done. Now on the coupler here, just start the sketch. Just create a line between this edge and this edge of the coupler. It should be perpendicular. As you can see, the perpendicular constraint is shown there. Just convert this line to a construction one because this is not the part of the assembly. Anytime while making the assembly, if you are losing focus of your sketch, you can always find it in the time line. Just right click here and addit sketch. Now from here, let's create a slot from the center point of the construction line that we have created. Let's say up to a distance of the center point of this particular coupler. Let the thickness be three and finish the sketch. Select this profile. Right click, press pull, just cut through. These two profiles have been generated. Now we need to cut this input link in this fashion. For this, we will select the input link. We will invoke the sketch. Now we are going to use a three point arc. Select a point in this edge, then select any prominent point that you want, and create a arc center. We need the same sketch over here. We need a mirror command for this, we need a mirror line For that, let's create a line from the center. Let's convert this to construction. Invoke the mirror command. Select this arc and for the mirror line, this construction line. And click on. Okay, I finish the sketch, select these two profiles by pressing control in the keyboard. Just shift and middle bows button to rotate or orbit. Basically, just press this one. Our assembly is officially completed. Thank you so much. 13. 14 Slider Crank Mechanism: Now the next assembly that we are going to create is quite a popular one. If you are from mechanical engineering background, you will definitely pinpoint its name. It's slider crank mechanism. Now, a slider crank mechanism is designed in such a way that it converts straight line motion to rotary motion. Rotary motion to straight line motion. There are many applications of this mechanism, like reciprocating Perms, rotary engines, piston cylinder regiment, and the list goes on and on. Let's create this particular assembly. Now for this we are going to have a different approach. We will create a component from the assemble tool bar. Let's name it Base. Then just create a box. We have box cylinder, sphere, Taurus coil and pile. These are the pre mat **** in Fusion 360. You can directly create them. Let's create a box on any of the horizontal plane, let it be of any dimension. Because all the assemblies that we're creating in the course, not two dimension. Now next we have to create this slider over this base, activate the head assembly, create new component, a slider. Then again select box, select this phase and just create a rectangular box. Click on. Okay, now again activate the head assembly. Let's save the file so that our head assembly can have a name. Let's name it a slider crank. As you can see, the name of the head assembly is changed. This is done to just avoid any confusions. Now, as you can see, the head assembly is activated, so both of the components are visible. You can move them around. Just revert the position, to revert it back to the original position. Now whenever I'm making any changes on any of the components, the other component might also get affected if it is getting in the way of the sketch. Notice whenever I'm going to make any changes in one of the component, the other component will also get affected only if the sketch and tities that we are creating overlaps with the other component. Let's say we are making a circular hole over this one. Let's select the midpoint of this edge and just create circular hole of let's say a MM diameter. Finish the sketch. Let's select the reason cut it through so that we can put a pin in this one. Notice the changes that we are making in this component is not making any changes on this component because the sketch entity is very far away from this one. But if this sketch entity was somewhere between this junction, then both of the component could have got this through cut. This we have seen in previous assemblies as well. Just press on. Okay, now let's switch to the next component. This is our stroke, but prior to that, let's create this particular pin. Go to Assemble toolbar, New component. Let's name it base pin. Select this phase, Invoke the circle command, let it be a MM. Only finish the sketch. Left click, right click, then select, press pull. Let's extrude it up to object. That means extend type two object and click on, Okay. Now from this particular phase, right click, press pull, let it be like ten MM only, and press okay. Now again, activate the head assembly and see if we have three components as of now. Now here let's create this particular stroke. As the name suggests, this component that we are going to create will define up to how much extent this slider will slide. Let's create a new component. Let's name it stroke. Now, from this particular phase of the pin that we have created, the base pin, basically, let's create a circular sketch entity, let it be of any dimension. Then trace this center point up to which you want the stroke. This defines the stroke length. You can change it to your choice, depending upon the length, to basically the extent up to which you want this particular slider to slide. Create one more circle. Let's make it a bit smaller as compared to the larger circle over there. Then join the outer circles with line command. Just keep in mind that tangency has to be maintained. Whenever tangency is not maintained, you can always look into this tangency constraint. Select the line, select the circle. Again, here also the line, select the circle. Now let's stream some unwanted areas. We are good to go finish the sketch like this profile, right click, press, pull that. It'd be like five MM in this side and click, Okay. Our stroke is also created. Next, we need a small modification on this slider component. What we will do, we will create a pin over this one inbuilt pin. Basically, we're not creating a separate component, We're creating something that is inside of the component, which is a part of the component. Just create it here. Just select this face and invoke the circle command first. Here, what we will do will create a center line from the center of this edge to the center of this edge. Let's convert it to center line from the sketch palette. Now from the center of this one, let's create a circle of let's say five Fm. Finish the sketch. Now here you have to make a certain geometrical adjustment. As we know we're having this particular pin protruding out by ten MM. We will create the pin over here which is not a component, which is the part of the slide itself more than this ten millimeter over here. Let's make it like 15 millimeter and click on. Okay. Again, the changes done in this component doesn't affect any other component because this was the sketch and Tity that we have created is not overlapping with any other component. Now the only thing that is remaining is to create a connection between this particular stroke and this pin. Let's create a connector. Select this phase, invoke the circle command. Let's create a circle, and then create outer circle that can have any dimension. But for the sake of proportionity, let's make it similar to the stroke one. Now here we have to make a certain adjustment. As we can see, we cannot pinpoint the center point. The center point is highlighted with a circular notation, which is visible here. This crosses are there, but it is not 100% show that this will be the centerpoint. What we will do, we'll go to create and project. This time we will project this particular sketch entity. In the selection filter you can see you can project bodies that we have done earlier in the earlier assemblies, and you can also project sketch entities of the previous component or the components that is hiding behind the shadows. Just click on okay here, because we need a sketch entity only, it will be highlighted. Now let's create a circle bigger than this one. And invoke the line command. And let's join these two. Do not forget to maintain tendency. You can see this tendency constraint. Let's click left click, that the tendency is maintained from here also. Now here the tendency is not maintained. Just click on tangent constraint. Select the line, select the circle, select the line, select the circle. Now trim some unwanted areas. Let's trim this and this and this, we are good to go. Just finish the sketch. Select this, select control, and select this one. Also, right click, press pull. We know it is like five MM more than this particular point. We can write five here. Our connector is also ready. Now the only thing that is remaining is to create a pin over here. For this, let's create a new component. Let's name it common pin. Select this phase, invoke the circle command. As you can see, the center point is visible with this circular notation. Let's finish the sketch. Right click press pool, and then extend type two objects like this particle surface and click on. Okay, finally, all the components are ready. The only thing that is remaining is to create joints and complete the assembly. As of now, we don't have anything rounded so we can move all the components. There is no joints, they are free to move. You can revert back to the original position by clicking this one. Or if you want certain different orientation of the assembly. Let's say you want all this over here, and here, and here, and here that you can see all the components. You can also click on capture image that if you make any changes and it will be reverted to the captured image that you have done. But we don't require that, just controls that. Now let's create the assembly for this. Let's ground this base. First you have to ground at least one component. Now click on joint, select this base pin and select the base. And let the motion be rigid. Again, create joint. You can press J, the keyboard as well. Between this and this pin itself, the motion revolute. Next, a joint between this common pin and stroke. Next joint between the common pin and the connector. Again, motion is revolute. Then between the slider and this connector. Again, revolute only. Finally, the most important joint slider. One, the slider select the edge. And notice that here the icon for placing the joint origin is quite fluctuating. You have to be very vigilant here. You have to see the orientation. The edge is perpendicular to the joint origin. That means you are good to go. But if it is not, your joint will be messed up. Always make it perpendicular like this, like this. Again, for the base, we have to do the same drill. As you can see, the slider joint is created gon, okay. Now let's try to rotate this. Yeah, I think we are good to go, but we need a slight modification because this is going out of the base. What we will do, we will just press pull it out. Now our assembly is fully complete. Just select any of the joint right click and limit the model to see the result. 14. 15 C Clamp: So far we have created some six to seven basic assemblies which involved rigid, revolute and slider joints. The Meserte of the assembly, all the basic assemblies that we have learned so far revolved around these three joints. Only now is the time to understand some intermediate assemblies that will involve cylindrical pin slot and planar joints. For this first we are going to cover cylindrical joint using this clamp assembly here. In this particular lecture we are also going to cover some additional concepts like motion link and contact set. These two concepts, the motion link and contact set will be covered comprehensively in advanced assembly. But just for the sake of understanding cylindrical joint, we are going to use it here as well. Let's begin. Just start a new design and create a component. Let's name it Frame. As you can see in the prevent assembly, we're having a frame. Then we have axle which is having a cylindrical joint and which will be rotating on the basis of the frame. Then we have a stopper, which is stopping it right over here. For this, for the frame component, let's start creating a sketch in a vertical plane. Let's make a center rectangle of any dimension. Then again, a two point rectangle. From here to, let's say somewhere over here. We are basically creating a frame like structure. Just finish this sketch, select this profile, right click, press pull, make it symmetric, this is too much, Let's make it five F. This is also, let it be ten only, and create the component, this is a frame component. Here, we need a hole to put the Xl in. Just create a circle trace the midpoint from over here from this edge to anywhere over here. Let's have its dimension as a whole number. Let's make it ten. Finish the sketch and just cut through it. Now we are going to provide thread to this one. Notice we are having this modeled option over here. When we are clicking on this modeled option, it is actually generating thread. That means if we are not switching this on this thread like structure is being made, but it's not actually a thread, it's just having a visualization of thread. When we click on Modeled, it creates actual threat. We are taking the thread profile as ISO metric profile StanMM, and designation as Ampton into 1.5 If you're aware with the thread nomclature, you will understand it pretty well. You can change it from here as well. Let's click on okay, our first component is ready. Okay, let's give the name to the head assembly. For that, we have to save the file. Now, activate the head assembly and create a new component. Let's name it X. From this phase, start creating a circle. We know the dimension was like teneM, but if we are seeing over here, it is not snapping anywhere to ten because we have already created thread. Means the dimension or the dimetrical position of the circle that we have created earlier has been changed. We will simply provide ten here. Click on. Okay, finish the sketch. Now you will understand what I'm saying. This, this blue coloration that is highlighting this whole circle. That is what we have created right now. But when we are selecting the region, this portion is being left out. This is because we have created thread beforehand. It's not the issue. Just press on control. This profile, this profile also. Red click, press pool, let it be up to this one. Let's make it two sides. And let's drag this portion just a little bit. Let's not put it over here because we have to provide stopper as well. Click on okay, basically we need this stopper in the end of the Excel and this handle at the other end. That's why we are not extruding it up to the surface. Now on this particular surface, let's create a rectangle, a center one. Then simply create a two point rectangle from here. Finish the sketch. All these profiles. Right click press pool just a little bit. Then let's provide fillets. Let's say here. All right, let's provide fill it here also. We are good to go. This created our second component, Excel. But we need to provide thread on this one also because thread is inside the hole as well. This thread that we are going to provide should have the same properties as the thread that we have provided in the hole. We'll go to thread. Yeah, this is almost same. You can also click on here to remember the size if you want. Let's make it modeled as well so that we can create actual thread perfect. Now, activate the head assembly and create a new component. Let's name it. Stop this we are going to create from this phase. Let's make a circle just a bit bigger than the diameter of the. Select this profile. Select the inside profile. Right click, press, pull. Now select this surface. Let's provide a taper of let's say seven degrees. This taper is not here in the pre assembly, but just for the sake of proportionity I have made, It looks good also. Now invoke the head assembly. All of our components are ready. How do we need to ground one component? Let's ground this frame one, capture the position. Now let's start providing joints. The first joint that we are going to use is between this and the center of the other side of the center of the hole. For this we have to select this plus sign over there. But for that, when we are dragging the mouse, it is not snapping to it. What we will do, we will press control in the keyboard and it will snap to it. But the motion here we are going to provide cylindrical. This is our first cylendrical joint. Let's flip the position, Everything looks good again. Let's adjust the position just for now. Let it. With this much, I think this is sufficient. And click on Okay. Now for the next joint, we are using the stopper and the Excel. Let's select this phase of the stopper and this face of the Excel, and let's make it rigid. And click on Okay. Now the assembly is fully complete, but some discrepancies are there. Like when we are moving this, it is not moving properly. It's having a very strange movement. Also we are having overlapping situation. Just revert the position. Let's make some adjustments. Here comes the concept of motion link. A motion link defines rotational and translational relationship between. Degree of freedom of joints. In simple words, a motion link defines motion of one particular joint with respect to another. In case of cylindrical joint, you can see there are two movements. One is a translation, that is the slider joint, one is rotational, that is the revolved joint. What is a cylindrical joint? Basically, cylindrical joint is a mixture of revolve as well as slider joint. What we will do, we will go to assemble and create motion link. For this, we will select the cylindrical joint icon, or here, since there is only one joint we are selecting, we will select this link with same joint. Now here you can see the distance is 100 MM and angle is 360 degree. This is saying that for the sliding joint or the sliding motion of this particular component, for every hundred millimeter 360 degree rotation, is there what we will do, We will just reduce it. This can be different. In your case, you had to have a trialon error method here. Let it be 50. This looks better. Let's click on, okay, let's rotate it. This is much better than earlier. Now let's address the second problem that is overlapping, reverse the position. One more new concept that is contact set. Just click on enable contact sets. You can see under the named views, you will see contact sets right click and new context set. And we will select this component and this component, that means they will not overlap anymore, they will have a contact. This is the beauty of contact sets. Click on, okay, Now we can move left words, but we cannot move right words. As soon as this contact happens. See, the same thing is here, also in the left hand, we cannot move it any further. Let's revert the position. That's it for our intermediate assembly, the first front cylindrical joint. In the next lecture, we will learn about pin slot joint. Thank you so much. 15. 16 Pin slot joint: Now let's create a pin slot joint as you can see here. For this, let's start a new design and create a new component. Let's name it Frame. Now, create a sketch on any of the vertical plane and create a center to center slot. It can have any length and any. Let's invoke the offset command by clicking in the keyboard and just offset it sufficiently. Click on, okay, finish the sketch. Now, select this region, press pull, and click on. Okay. Now create another component, Let's name it Slaughter. For this one, select this particular phase, create a circle. Let's snap to this, finish the sketch. Just extrude it outwards. Click on Okay, then select this surface. Create another sketch again, a center to center slot. Select this, it can have any distance. Finish the sketch. Select this region. Select this region also by pressing control and press for it outwards. We are all set to create the joint. Just invoke the or activate the head assembly and go to joint. Now select this particular phase, this particular joint origin for slaughter and for the frame. Just hover the mouse anywhere and select the center by pressing control and just flip the position. The motion type is pin slot and click on. Okay, let's animate the model. You will see some overlappings there. What we can do, we can simply edit the joint limits for rotation, there is no issue. We need to edit for slide, let the rest position be zero MM only for maximum. Let's say 20, Better make it 25 or even 30, minimum. Let's make it -30 We are all set. Click on okay, and animate the model. This is how a pin slot joint is created in Fusion 360. Now you might ask, what is the difference between a cylindrical joint and a pin slot joint? For this, we are having a assembly that we have made earlier here, what we had when we are rotating this handle, we are also having a sliding movement. But as you can notice, this rotation and this sliding motion, that means the rotational and translational motion is in one axis only. Let's show the joint. Let's see the cylindrical joint. Just click on added joint and you can see the motion. The motion is in axis only. But in case of the pin slot joint, when we click on added joint, you can see in the motion for rotation we are having Jad axis, but for sliding we are having X axis. That means rotation is in one axis and the translational motion is on another axis. That's the basic difference between a pen slot joint and a cylindrical joint. 16. 17 Creating a curved slot: So far we have understood about rigid joint revolute joint and slider joint while we were creating some basic assemblies. And then we understood about cylindrical and pin slot joints while we were creating some intermediate assembly. In the same regard, we are going to understand the planar joint and the ball joint. This ball joint will be covered in the next section. We are going to deal with some advanced assemblies and some advanced concept of assembly in Fusion 316. Let's begin with this one. As you can see, we are having a curved slot in which a pin is attached, which move in the slot only it cannot go outwards. Of this, we are going to use the concept of context, set again here. Now, in this particular lecture, we're not only going to understand about the planar joint, we're also going to understand about one new concept, that is how to create a joint origin. Let's begin. Let's create a new design and a new component. I always start with a new component from the assembled toolbar. I can also do it by creating a body, then creating that body as a component. But this is more convenient, this is more prominent, and this is more efficient. That's why I use this. Most of the designers use this method only. They create components, a fresh component, from the assembled tool bar. Let's create one, let's name it slot. Now we are going to create this card slot first for this, create a sketch in any of the vertical plane, then create a circle of any dimension, a bigger one, and then followed by a smaller one. Then invoke the line command. Tress the origin up to the intersection point that we are getting here with respect to the outer circle. And then just close the region. Let's trim the bottom area. This one. Also invoke the offset command by clicking in the keyboard. Just offset this profile that we have generated outside and click on Oki. Finish the sketch, select both of these regions, press pull it outwards, let it be of any dimension. Then as you can see, the sketch is gone. What we will do, we will show the sketch from here, from the browser. Now select this outer region, press pull this time here operation would be obviously joined. Now just hide the sketch. Our slot is ready. Now we need to create a Pin over here for this. Again, invoke or basically activate the head assembly, create a new component, Let's name it Pin. Select this particular surface, create a circle. Let's first create a line from this midpoint of the curvature and this midpoint, let's convert this into construction, one from the center of this one. Let's create a circle. As you can see, it is snapping to the point with the outer Dia of the Cod slot. But this is not desirable. We need to make it s the reason behind the same is we need to have a play in between them. Otherwise it will be stuck. It is like 37.36 millimeter. We can make it like 36 so that we can have play in the upper portion as well as in the bottom portion. Clkana and fringe, the sketch, this profile press pool. I think this much would be sufficient then from this face create another circle, a bigger one. Finish the sketch, select both of this profile, right click, press pull. We are done. Now in this assembly, both the components are ready. Now we need to ground any one of them. Obviously, this slot is going to be grounded. Let's capture the position. This is grounded. That means we cannot move this one, but we can move this one. Now, apply joint. Which one? Planner? Let's go to position snap to this particular origin. Joint origin. Then you need to find a point to snap it on the slot. But as you can see, there is no prominent point where we can snap. Let's say we are snapping it here. We are trying to adjust it, but it is not going to be adjusted properly. Now what we need here is we need a joint origin where we can create a joint between the components for this go to joint origin. Basically, the description in fusion itself is telling you that a joint origin positions a joint origin on a component which defines the geometry used to relate a joints component. That means when we define, when we create a joint origin, it will create a new origin where joints can be applied. When we invoke the joint origin Scpture, the position we have mode simple, between two phases and between two edge intersection. When we try with the simple one, we cannot snap it to any prominent position. We have to try something else. The second mode is between two phases. When we click here, we can select two phases only, but we want our joint origin somewhere over here. For this, we need to make some adjustments. Just cancel for now, and create a tangent plane on this particular curvature. Similarly, create a tangent plane on this particular curvature. Cliconoka. Now we can invoke the joint origin. Just select the mode as between two phases, Select this phase and select this phase. And we can provide joint origin in between these two phases. But as you can see, it is not oriented properly. It should be lying parallel to this particular surface. For this, we can click on Reorient. Then for the Jad axis, we can select this particular surface and it will be oriented properly. Click on, okay, Just hide the constructions. Now we can provide the planar joint properly. Just go to Join For Motion. It's we have selected it earlier now for the position to Snap would be this one and the new joint origin that we have created. Now as you can see, this is how a planar joint works. Let's click on Animate. What a planar joint does is that it moves the component along with the plane in which the joint origin is. It is moving it around the plane in which the joint origin was made. Joint origin was made in this particular plane. It is moving in that plane only. Let's revert the position. But what is desirable here that it should move under this slot only for this, we will again use context sets. Just enable the context sets. Right click here and create new context set. Select both the components and click on, okay, now when you move the pin, it will not go outside of this slot. 17. 18 The Ball Joint: Now we're going to start with some advanced assemblies in which we will understand about ball joint. First, let's make this assembly to understand this. This is like a joystick. If you have used or played games in your PC, you must have seen this moment there. Even in your consoles of 4.5 this movement can be noticed. Let's make this assembly. We will begin with a new component. It can have any name, there's no issue with that. Create a sphere on this particular horizontal plane, just involve the origin. Let's make it like 60 M and click on. Okay. Now create a sketch on let's say this plane, a two point rectangle. Then just press pull this one symmetrically and the operation would be cut. Now invoke the shell command from the modified toolbar. Select this particular surface. Let's prod shell of any thickness. Let it be one on it can be different in your case. Now our first component is ready. Let's activate the head assembly and create another component. This time also let's create a share on the general plane and select this origin. The larger sphere was 60 MM. Let's make it a bit less than that. Let's make it like 57 MM, and click on Okay. Again, this dimension can be different in your case. Now, create a sketch on the original plane. Let's create a circle from the origin. Finish the sketch. Let's hide first component, let's hide the body of this one, the second component. Now select this particular profile sketch profile that we have created. Show the body of component two. And show the body of component one. Right click, press pull. Let it be outwards. Let's make the operations join. Click on, okay, let's create a sphere on this particular surface. Let it be 15 MM, and operation should be join. Click on. Okay. Now let's provide fillets on this and this face perfect. Now activate the head assembly and both of our components are ready. What we will do, let's capture the position first what we will do, we will ground this one. This is sphere in which we have created a shell. This is acting as a outer sphere. Let's ground this one then go to Join in the motion. Select ball joint. For position, you have to just select the surface of the sphere. Anywhere you can click for the second component. For this one you can click anywhere in this share, but you must not click on this particular surface. Otherwise the joint will be created here. I'll just click it and press Okay. Now you can see the movement that we desire has been achieved, but there is overlapping between the components. For this, we all know what we can use. We have been using it for some time now that is contact sets. Just enable contact sets. Right click here. Create a new contact set between these two components. And press okay. Now you will see that it will overlap. The components will not overlap and our ball joint is complete. 18. 19 As Built Joint: Now in this particular lecture we're going to create a assembly using as built joint which basically positions components relative to one another. And then it creates a relative motion between them. To demonstrate the same, we're having this cam and follower assembly over here. Let's animate the model. We are going to create this particular assembly purely using as built joint. Let's begin with a new design. Now, here in the premed assembly itself, you can see we are having four basic components, this follow shaft and this base frame. We will be using the same procedure, creating components one by one relating to each other. First we're going to create, let's save the file so that we can have a name for the head assembly. Let's name, it can follow. Now, to create this particular component, we need to create a sketch in one of the vertical plane. Then we need to create a circle of any dimension, followed by another circle which is inside this one, and then a smaller circle. Basically what we are creating, we are creating this particular profile. Now let's create another circle by tracing the origin somewhere over here. And its diameter should be equal to or a bit less than this one. Let's make it tangent to the outer circle. Now invoke the line command. Select anywhere on the outer circle and then maintain the tangency till this newly built circle. Same thing here as well. Now, invoke the tangent constant. Select this line, select this circle. Again, select this line, select this circle. After that, invoke the rectangle command. Center rectangle, select this center point and create a rectangle like this. Just delete these construction lines of the center rectangle. Invoke the trim command. All the unwanted areas, we are good to go. Now here, select this profile. This one, This one, and this one. Let's press pull it symmetrically, let it be five mm. It can be any dimension operation would be new body and click on. Okay. Now as you can see, the sketch is gone. So we can always show the sketch from the browser inside the component, that is the cam. Just click on here, or you can just select this and press V in the keyboard, the sketch will be shown. Now select this profile, right click, press pull again, symmetric, and this time we are going to extradit outwards like this. Let be seven MM, I want to extradit two MM outwards on click on operation was join our first component. This cam is created, just hide the sketch, activate the head assembly and create a new component. Let's name it follower. Now for this one, we have to select the origin. Again, just to show the origin. This is very light in coloration. You have to be very vigilant here. Select this particular plane on which we have created the earlier component and then create a sketch. Now we need to project this one. Press in the keyboard selection filter as sketch entity and click on, Okay. Then invoke the circle command, trace the origin and find a prominent point somewhere over here. Let it touch the projected circle and the tangency is made. Now here again make a small circle. Invoke the rectangle command. Two point rectangle this time. Trace the center point of the circles that we have created till the inside circle. And start the rectangle, let it be sufficiently long, then use the coincident constraint. Select this point in the rectangle and then this circle. Now the length of this follower depends upon the stroke length. That means this distance, this particular point to this one. Let's measure it. It is like 60, 1 millimeter in this case. Let's measure our follower. It is just almost double the dimension that we have seen. Basically double the stroke lend. This is the most prominent way of making a man follower of this type. Because as you can see in this particular pre assembly when we're animating the model, the follower is jumping upwards up to the stroke length. The stroke length between this point to this curvature over here, the follower has to be made sufficiently longer. Now just edit the sketch again and let's trim the unwanted areas. Now we have to extrude this particular profile and this one as well. Let it be symmetric. Only select this surface, let's make it a little bit less. And click on. Okay, now show the sketch this time. Select this profile, hide the body, and select this profile. Show the body, right click, press pull again, symmetric up to this surface. Let the operation be new body. Click on. Okay, now our follower is also ready. Hide the sketch and activate the head assembly. Next, we need to create this particular shaft followed by this frame. For this, create a new component. Let's name it Shaft. Now for this one, we need to extrude this particular profile. What we will do from this surface, we will create a sketch. Then we are going to project this complete region. Press in the keyboard, select this reason, press anywhere in between here, then click on Ok. Now finish the sketch. Select this profile, right click, press pull up to this surface. Click on, now create a cylinder on this extruded surface. It will snap to the centerpoint and then it will snap to the outer point. Let's give it some proper dimensions. It can be anything. In your case, let the operation be joined and click on. Okay. This here created our shaft as well. Now the only thing that is remaining is to create this particular base, which is joining the shaft to the follower. For this, let's again create a new component. Let's name it Base. Now for this particular base component, we need this plane. Create a sketch on this plane project. This particular body, that is the body of the shaft. Then anywhere here, you can create a two point rectangle. Invoke the line command. Now, from the centerpoint of this created rectangle, let's start drawing a vertical line. Let it be sufficiently long, then a original line, we should be close enough to this particular surface of the follower. It should not be touching it. Create a fill it over here. Finish the sketch. Select this rectangular profile over here, and create a revolve for the axis. You can select this projected Diskatchlkonok. The sketch is hidden, so we can show it from the browser. Now for this profile that we have created, we are going to create a pipe for the path fell. Select this. Section is circular, but section size is very large. Let's reduce it to like ten men. You can also make it hollow if you want, but better make it solid only. Then click on Oka. We have created this part and this part of the base. Now we need to create this particular part for this, just construct a plane at angle and then select this line o, this is the line which we have used to create the pipe, but this can be used for creating a angular plane as well. But we don't want any particular angle, we just want a plane over there which is cutting the pipe in between. We will provide the angle as geodegree only and click on. Okay. Now on this surface, start creating a sketch just for convenience basis. Hide the cam component and the shaft component so that we can only have the follower component visible. Obviously the base component. Now project the body of the follower component, this has been projected to the sketch, and also project the body of your base component. Now create a rectangle. A rectangle, Select the midpoint of the followers projected diskatch. We can find its midpoint centerpoint. Then place it so that it is touching the projected diskatch of your base. This much is sufficient. This looks good. Select this profile, right click, press pool, make it symmetric. Just give it a glance if it's covering the pipe or not. Let's extra somewhat more operation is join now let's if an extra bodies are there, we can see that we have two bodies. What we can do, we can use the combine command, Select this one, select this one, let the operation be joined. And do not check Keep Tools option here. Otherwise it will create a duplicate body. Click on okay, and now we have a single body inside the base component. Now the only thing is remaining to create the assembly, but for this we need to ground at least one component. Let's ground the base so that all the other components are free to move. Let's revert the position now. To create the build joint, you have to go to assemble tool bar. You can click on as Build joint or you can use the keyboard shortcut shift plus J. Let's invoke this one. Then select two components. Let's select the shaft and then the base, the joint type would be revolute. Then you have to snap to one point. You can either snap to this particular point of the shaft, or you can snap to this point. That means either of the ends. Let's snap here. We have created a relative motion between two components. Just animate it and see this is the desired motion. Just click on. Okay. Next we need to provide a relative motion between the Cam and the shaft. So that the shaft and the cam accordingly revolves altogether. That means when we are rotating the shaft, the cam should also rotate or vice versa. For this, again, we will invoke the spill joint press shift plus J in the keyboard, select the Cam, and then select the shaft. Let's provide the motion as reside. As you can see, the cam and shaft are rotating along with each other. Let's see what the position then we need a relative motion between the follower and the base. Let's see the moment in the premed assembly so that you can have a clear idea what we are doing, why we are creating these joints. Just animate this one and see this is the desired result. Here we need a slider joint between the follower and the base. Again, go to S build joint, select the follower followed by the base. Let's provide the joint type as slider, then select the snap point or snap surface or snap edge. As this one we can have a slider motion between the base and the follower. Now when we rotate the cam, this follower is supposed to go up, which is not happening as of now because it is overlapping. Revert the position and use the same command. Use the same procedure that we have been using for quite some time. That is, contact sets just right click, provide new context set between the can and the follower. Let's select the bottom body because we are having two bodies in the follower. Click on. Okay, now let's animate the model. All right, as you can see, the follower moved along with the cam, but it got stuck in the top portion. What we need is to provide joint limits to the slider. Just click on the rest option to zero MM and click on Okay. Now animate the model. We have achieved the desired result. This complete assembly was made with as built joint. We have not used the simple joint anywhere. 19. 20 Motion Links: Now they are just a couple of things that are remaining in assembly. Motion link, tangent relationship, and motion study. In this lecture, we are going to understand about motion link. Now for this, we are having this warm gear assembly where when we rotate, the warm, the gear rotates accordingly. We are going to create this assembly, but we are not going to make anything. We are going to use Mac Master Card component. From where we can import these components directly into Fusion 360. Just click on inside toolbar. Go to Macmaster Car component, then you can find a list of varieties of components available which you can directly import into Fusion 360. And you can start working on them directly, but for this particular lecture, we need to find gear inside gear, we need warm gear. Let's select this. Metal worms and warm gears. Now here we will first import a warm width Kat bore. Let's select a 12 pitch or just click here and select three D step. Just reson download. There you go. You have your component ready component. Basically you don't have to create anything. You can directly import it from Mcmaster Car component. Now next we require a gear corresponding to the worm only. We will go to gear, metal worms and warm gears. Then we will select a gear. We have selected a 12 pitch worm. We will again select here a 12 pitch gear. Let's select this one and download it and just make sure this is step. Our gear is also imported into Fusion 360. Just rename them, This one is warm, this one is gear. Now we have to make some slight adjustments. As you can see, they are overlapping. Just click on the warm. Invoke the move command by pressing M in the keyboard. Just drag it upwards to some distance and rotate it by 90 degrees. Now we have to adjust it so that the teeth of the worm gets in between the ***** of the gear. For this, again invoke the move command. In move object, you have to select component. Because this is a component, this is not a body. Select any point anywhere, then drag it downwards a little bit, right? I guess even with precise hands, cannot be sure that there is some interference between the two components. For the what we will do, we will go to inspect, selecto interference, capture the position, select this, select this. And let's compute. As you can see, there are some interference over here. We have to adjust them. This is like a trial and error method. You have to adjust it using the move command, obviously. And then you have to again, recheck it until and unless you're getting the interference as a zero, you cannot move forward. Just click on. Okay. For now, let's move it by, let's 0.2 Let's again check it. Like both the components and compute. You can see steel interference is there. We are going to repeat the process until we are getting Jio interference. We are going to fast forward this particular section. As soon as you get this no interference detected notification, you are good to go. Just click on okay and cancel this one. That means there is no interference between these two. Now we're going to learn a new concept. Let's create a new component. Let's name it Axis Cliconoka. Now for this new component, we're not going to create any three model. We're just going to create from the construct tool bar A axis through cylinder, Cono, Taurus. Then we will select this particular profile of M, then Clonoka. This particular component will only have this axis. This component can be regarded as a pseudo component because it is not having any geometry, any sketches, any theory model. But it is still a component. We can use this component, this axis basically, which is converted into component for providing joints. Now let's provide joint between these two. We are going to use again the as bill joint just like we have used in the previous assembly press shift plus J in the keyboard. Select this component and select this pseudo component which is just a axis. The joint type would be revolute and snapped. To this point you can see a rotation of arm is seen. Let's click on, Okay, let's do the same thing for this one. Also just create a new component. Let's name it Gear Axis. Then again create axis through cylinder otaurus and select this profile. Click on Ok. This is yet again a pseudo component, a false component. Again, invoke the head assembly. Invoke the as well joint. Select the gear and select this pseudo component, this axis and snap. Let's say this point, this one is also revolute. Click on. Okay. Now what we need, we need a relative motion between these two joints that when we rotate, okay? This is moving freely. We need to ground something again. We can use these pseudocponents to ground them. Let's ground this. This can move, this can only rotate. Is this one moving? Yes, this one is also moving. Revert the position and ground this pseudo component. Also both the pseudo components that we have created, the axis that we have created as components are grounded. Now what we need as soon as we rotate the form this gear below should also rotate accordingly. We need to provide some relationship between this revolute joint and this revolute joint. That relationship is what we call motion link. Just click on motion link here, select this joint and select this joint. As you can see, we can have a relative motion. Just click on, Okay, this was your motion links. Now coming back to these pseudo components, we can hide them. They are like they were never here. But they did the work. They did the job of providing the motion link. 20. 21 Tangent Relationship: Now the next thing we're going to learn is tangent relationship. Now as the name suggests, it creates and maintains a positional relationship between a phase of one component to a phase of another component. This positional relationship between the phases is tangential in nature. Now to understand this particular tool, we are again going to use this Cam and follower assembly. This premade assembly we have made this assembly to demonstrate how to use as bill joint. If you can recall in this one, what was our main motto? Our main motto was to create this particular movement of the assembly. That means the follower is eventually revolving around the can. To create this particular motion, we needed a contact set. Then we had to, if you can recall, adjust this slider joint by providing joint limits. It took like two to three steps to create this particular motion, but with the help of tangent relationship, we can simply select phases of respective components to create this motion. Now to understand this one, let's delete the context set by clicking here. Then in the context sets, you have to disable contact for the slider. Let's uncheck the rest option. This is like a normal assembly with no contexts. That means when we animate the model, the cam will be overlapping with the follower. Now we are going to use tangent relationship for this. Just click here in the assemble tool bar. Then you have to select phase of one of the component and then phase of another component. Let's select this one and click on, Okay. Now let's animate the model and see this is also generating the same result, but with lesser steps. 21. 22 Rigid Group: Now the next concept in assembly making is rigid group. This rigid group locks the relative position of the selected component, and then those selected components acts as a singular component. In order to demonstrate this particular concept, we have these four components over here. This base component, this one is grounded already these three other components. Just for the sake of demonstration, we are going to make this assembly the position. Now here, what is desired is that when we rotate this particular component, which is in the middle, these two components should revolve around this circular slot. Now to achieve this assembly, we can always provide individual joints to all these components relative to this grounded component. Then we can provide motion link in between them. But that procedure will take like four to five or even six to seven steps to do so. Here comes the role of rigid group in these situations. We can use side groups to make these three components as a singular component and provide respective joints in the respective motion. Let's do this and understand the concept of Sid group. Just click on Assemble tool bar followed by Sid Group. Then you have to select the components. Select this middle one, this one, and this one, And click on, Okay. Now, as you can see, when I'm dragging out any of the component, all the three components are moving all together. Let's reverse the position when we provide a revolute joint between this middle component and this grounded component. These two other components that are a part of a rigid group will also have a revolve motion around this circular slot. Let's do this, provide the joint shortcut for the same is jam the keyboard. Select this one for the grounded component. This one click on. Okay. You could have also used as Bill joint if you want. Now when we rotate this, the other two components are perfectly revolving around the circular slot. That's the beauty of rigid groups. This can be utilized in many scenarios. It's very useful in assembly making process in Fusion 360. 22. 23 Motion study: Now the only thing that is remaining in the assembly making process is the motion study, which performs kinematic motion analysis based on joints. Now to understand this, we're having this Cam and follower assembly in which when we animate the model, you can see the cam is rotating and the follower is moving up and down. Now if I want to demonstrate a complete rotation of the Cam followed by a reverse rotation, this would not be possible just with animating the model, because when we're animating the model, it is only rotating in a clockwise fashion. Here we can utilize motion study. As soon as we click it from the assembled tool bar, a new pallet opens. Just adjust your model accordingly so that you can see this pallet, and you can also see your assembly here. As you can see, there is a straight line. This line is eventually axis of time. If we consider this axis as X axis, then in the Y axis, we can consider positional antities like degrees, millimeters, or basically distance. Now on the right hand side, you can see this joint revolute joint is already selected. You can always deselect it and select any joint you want. But for the sake of this particular lecture, let's go with the revolute only. Now here as we drag the mouse, you can see the numbers are changing. These numbers are what we call steps. Now let's select any step. Let's say we're selecting this step number ten. As soon as we selected that by left clicking on it, you can provide angle. Initially what I told you, that I want a complete revolution of the Cam followed by a reverse or anticlockwise revolution. Initially, I want a complete clockwise revolution and then anticlockwise revolution. Here I can write 360 degrees. Just press anywhere. Let's say at step number 50, I am reverting it back to zero degrees. Click anywhere again, just click on Play over here. This was very fast, but when we play on Loop by clicking here, you can see the desired result is obtained. A complete revolution followed by a complete anticlockwise revolution. You can also delete any of the points that you are created in the graph by clicking this minus sign over here. You can also create a smooth operation by providing larger number of steps. Let's say we're providing, instead of 50 steps, let's say we're providing 90 steps, let it be zero degree. When we click on Play over here you can see rather smooth operation in the reverse direction, or the anticlockwise rotation is seen with this, we're going to conclude this course. I hope you understood the in and out of assembly making process in fusion 316. I hope you will apply the knowledge you have gained and you will create your own assembly in no time. Thank you so much, all the very best.