Welcome to the next video and our Disc Golf 3D modeling series. In this video, we're going to model a chain using in context assembly features and curve patterns. In the end, we're going to use SolidWorks motion analysis to examine the shape of the chain under gravity. Let's get right into it. First things first. We're going to create a sketch on this assembly level, which will help us make the chain onto this hook. So this will help us, parametrically link the geometry to our mates. So if anything ever changes down the road, the mates will update accordingly. on this point, here is where the chain hook is going to be mounted. And we're going to be using this point as well later in our motion study as our initial position for the hook. And we're going to just quickly rename the sketch because it's important to be organized in our feature tree. And the sketch is going to be our outer chain hook mount. Sketch geometry. Let's drag in the hook directly from File Explorer. We can choose the configuration. If we chose the wrong configuration initially, we can always change the configuration on the fly from the feature manager tree. There we go. And now we can position the hook in place by doing a quick left click and drag. We can move the component in 3D space with the right click and drag. We can rotate that part and get it ready in its, orientation for mating. There are many different mate types and works. The first one we're going to use is the coincident mate between two different points. And then we're going to remove this degree of freedom from the part by mating two sketch lines, parallel to one another. And then we'll have one more, degree of freedom, which is the rotation about the axis. We'll take care of this by mating two different planes parallel to each other. Just like that. And now the hook is fully defined in space. Next, we will insert a new part into this assembly. We'll give it a name. Outer chain. And now SolidWorks is asking us which face or plane. Do we want to insert this part on? It's going to establish the origin. So we're going to click the front plane. Now we can see in our feature tree we have the part called outer chain. And the origin matches the assembly origin. And we can continue modeling from here. So we're going to create the shape of the chain based on the hook and the chain ring below. So we're going to use the geometry of the assembly to create our shape of the chain. And this is true in context assembly Modeling. It's called modeling from the top down which has been described in the previous article and video. So we're going to take the geometry from the chain ring, convert it to construction and then we're going to use that as, an anchor point for our spline, which is going to start from up here. We're going to first start with a line segment coming off of that sketch point from the hook, and we're going to dimension it. It looks like we didn't quite grab the top point. That's okay. We can, double click or control click both points and then meet them using sketch relations. So we're going to make coincident. And there we go. It's fully defined now. And next up is to add the spline. So we're going to approximate the shape of the chain hanging here the sketch. And then later on we're going to simulate the shape using SolidWorks motion analysis. Now that we've made a tangent relation between the spline and the line, we're going to go ahead and add a dimension to a spline. Yes, you can add dimensions to splines and SolidWorks. And this is very helpful for wiring or even, you know, knowing the linear length of your chain, you can apply it through the dimension of a splint here. Now we'll switch over to the part. And as you'll see, because we modeled or sketched the geometry in the context of the assembly inside of that part, we do have that sketch in the part here. So we can start sketching the first link. And we're going to use the slot tool to do that. There's different dimensioning schemes available for slots. So for the width wheel, smart dimension, the width, just like that. And then we will dimension the center, distance of the slot by grabbing that line. If we want the overall dimension, the max arc arc dimension, we can go into the leaders tab and then choose the max to max. Dimension style. All right, there's the length of our slot. And now we're going to make that slot to the beginning of the chain. Because we're going to be doing a sweep. We need a sweep profile. Now we're going to add a sweep profile, a circle profile to the edge of the slot. And we're using our s key to pull up our most commonly used tools. We're making the easy job of sketching this circle here. We'll go ahead and sweep the profile along the path. And there's our first chain link. Solo works has a bunch of tools to make us more efficient in our modeling. So instead of drawing all of those sketch profiles again, we're going to use move copy bodies to create a copy of this body. And we're going to translate it down in the Y direction. And then we're going to rename the feature in the tree so we know what's happening there. And then we're going to do another move copy bodies to rotate the body. This time we won't copy it because we want to move this body 90 degrees. And now we have our 90 degrees alternating chain. Next up we need to make a pattern of these bodies along a curve. So to do that in this instance we'll need to create a curve based on the sketch and then activate curve driven pattern. Select the curve. And then we can choose of the bodies for patterning. So both of these bodies will be patterned. And we're not seeing the preview because it's showing up as an edge in the selection box. So we want to make sure that in this scenario we select the curve from the feature tree from the flyout feature tree manager. And now our preview is showing up. As expected there are many different options such as the spacing, the number of instances, whether you want equal spacing along the curve, curve method, alignment method instances to skip similar features and options that we see in other pattern tools, in SolidWorks. But there we go. Our chain has now been, patterned, and we have a full chain. We can go back to the assembly and check out our result. And as you can see, we have, some issues here. We have overlapping geometry and bodies. So we're going to go ahead and fix that up. Or we'll jump back into the part file and we'll change some parameters. All right. That's looking a lot better. But it does look like we have one extra chain link. So we'll fix that up. To do that we'll we will use the delete key bodies feature, which allows us to remove a body without, destroying it forever. This is a reversible move. As it shows up in the feature tree and there we go. There is our completed approximated, chain assembly in SolidWorks, with the outer chain. Then we'll follow the same steps to finish off the inner chain. And then all that's left to do to complete the assembly is to create a circular pattern about this, axis here. Now let's move on to the simulation motion analysis. Part of the video. I've created a new assembly called this Golf Assembly Dash gravity. And it's typically a good practice to create either a new file or a new configuration for your simulation studies. And that's because each study might require a different setup of your feature manager tree. Or you might need to simplify your parts down. So it's a good practice to do that. For motion analysis, we need all of the parts at the top level, which is why we've dissolved the subassembly for our chain parts and shoved all of the bodies into the outer chain parts folder, as you can see here. And they're all under under defined, which is fine because we're going to establish the, pair contact in motion analysis. And then gravity will take over from there. To enable motion analysis, first we need to make sure our addin is checked on for SolidWorks motion. And then in our motion study tab and the list will have motion analysis which is the most realistic simulation. It takes into account all types of motion objects and provides accurate simulation based on numerical methods and fully physics based basic motion is not quite as realistic, but it has its use case for simple motion analysis, where realism isn't as important. In this case, we're going to use motion analysis. We've set up the contacts. As you can see here. Here's a list of all of the, parts that are participating in the contacts. So, motion will see these and create contacts between them. We increase the friction to one because we want this chain to settle down as quickly as possible. We want the motion to dissipate into heat. And then we also, change the elastic properties of the material, increase the max damping also to, settle down this chain as quickly as possible. As you can see, the chain is inserted as a linear straight line. And then gravity will will exert force on it. Accelerate all the links down and it's going to take on this shape that we're looking for. We've also added gravity pointing in the negative y direction. And that's about it. There's no other, options or features that we've added here. We can just click calculate. This will run the solver. It'll take some time depending on the complexity of your study. Then you can, change the speed of the playback and playback your animation like so. We can see our chain settling down in its natural state. So I hope that was, valuable insight into motion analysis. And we're going to continue working on this model in the next video. So we'll see you there.