TriMech has partnered with the Disc Golf Pro Tour, and we'd like to show you a way to model a Disc Golf Assembly Basket using SolidWorks with a top-down approach with a skeleton sketch. Here's my finished assembly, less the chains, which will be modeled in another video. But for this video, I'm going to be working with a top-down modeling approach that I'm going to show you. This is really useful when parts are tightly related, share design intents, make sure that everything fits together nicely, versus the more traditional bottom-up approach where individual parts are designed separately and then brought together in an assembly. I'll go over some of the pros and cons of this method at the end of the video. You can see here we've got our full assembly, and then I have access to a master sketch where I can update the entire assembly as one item. So let's get into designing this assembly. So how do we build this? In this case, I have a reference master sketch. This is going to be used for everything. In this case, as you can see, I have almost the entire design inside of one sketch because pretty much everything is simply revolved or patterned from this sketch. I have my support, I have my basket, and I have my top deflector. And what I have here, these dimensions are the values in centimeters from the pro guidelines for a basket frame. But I could also put these in as equations, as global variables as well. But it's kind of nice in this case to have them so I can just edit them right inside the sketch, as I'll show you a little bit later. So how did I model this? I've got a sketch here showing the inside of the basket, some of the rings that we've got. And then this simple sketch along the outside is going to be for the outside wrapper around the basket that's going to be patterned. And so just making a simple line with half of the diameter of that part will allow me to very easily model that. So I've got my master sketch there. So I've got my master sketch there. And I've also got another sketch for the larger ring that we're doing. Once I have that sketch done, what I can do is start making the parts. And I can insert a part and just insert that reference master sketch into each one. In this case, I can just grab mainly the sketches. So I've got this. And now what we're going to do is we're going to make this top part. And I can do a revolved base where I grab that master sketch, grab my axes from the sketch, and then get the contours that I want. I've got three main contours for the main part. I could also break this into a sub assembly, but in this case I want to have it nice and simple as a multi-bodied part. So I've got these parts made. I can now go ahead and simply do a sweep again of this sketch. I had my diameter. And then I've got that part. I can go ahead and pattern that again. Using this sketch center line. And then instead of a feature, I will use a body. So I can pattern this body. So we've got our 12 here. And then as I mentioned, we also have this one. We can do another swept boss for this part. I'm going to grab that sketch. Again, it's a quarter. Pattern this body. What we're going to have here. What we're going to have here is 12 inner chains and 12 outer chains on here. And pattern that. And so now we've got our part done. We'll put some material here. I'm going to use a galvanized steel. All right. So we've got that. Now let's apply a color. In this case, I'm going to use a solid blue. The part level. So that's looking pretty nice. As a final touch for the deflector, I've simply made a text on the front plane. And now what I can do is a wrap. Choose this surface. And now I've got a nice trimac on my deflector. And then create my next part. One thing we can do is that have solid bodies for this. So if you simply put this in a drawing, you're not going to get a bill of material. But you can make this a weldment. And cut list is automatically created. And then your drawing put in a weldment cut list. And that'll get all of 12 of these parts. So I've created my next part. I have my material. I have my sketch inserted. I can go ahead and do my revolve again with the specific contours. And now I did a sweep of this part. And I patterned it again. And I've got my basket done. All right. So I've made my disk support with the same technique and the disk pole. So now I can go ahead and assemble these. And the nice thing is that it's going to be a little easier than normal. So what we're going to do is insert our sketch first. And what we can do here is change this to an envelope part so that it doesn't show up in a bill of material. And then the other thing we can do is we can add our sketches to favorites. So inside of the assembly, I'll be able to modify the entire structure. So now we have our main sketch. We can start inserting components. Let's start with the support. A new feature in 2024 allows us to automatically fix or float components going forward. And in this case, I want them to be able to be fixed because they're all based on that sketch. And so I can bring that in. I can repeat. For the disc pole. Have that fixed again. Bring in the basket. Again, simply have that fixed. And bring in the deflector. So I've got my main assembly. I'm going to turn off my sketches right now. And we are done. So now I've saved my assembly. And we have completed our design using a top-down modeling and skeleton sketch. So I've got my master sketch here. I can go here and make whatever updates I want. And what that's going to do. That's going to update my assembly. All of my parts, my assembly, the location of everything. So this top-down skeleton model with a master sketch can be a really nice way to design in SOLIDWORKS. So thanks so much for watching me create the disk golf assembly basket in SOLIDWORKS. So this is a really nice way to design in SOLIDWORKS.