Transcription
Hey there everybody. My name is Gabe, and I design 3D printable action figures. In this mini tutorial, we're going to model a basic ball joint in Fusion 360.
Ball joints are sort of the basic building block for an action figure, so I figure it's a good place to start a little tutorial series. We're going to model this segment here. It has a ball on one end and a socket on the other. You could print two of them, connect them together, and you're like halfway to an action figure right there.
So let's jump in. I'm going to start a new design. I'm going to save it. I'm going to call it "ball joint." Now, before I even get into sketching, I'm actually going to go to Modify, drop that down, and go to Change Parameters. So if you haven't worked with parameters before, they're actually really useful. You can basically set stuff up in here that you know you might want to change later or reference later. And then rather than going back and digging up the original sketch that you did something in and editing it directly, you can just change the parameter in this menu. And if you set things up right, uh, in your modeling process, it will just update the model on the fly with the, uh, new parameter value.
So I'm just going to click this little plus to create a new one. And the only parameter that I'm actually going to set up is length. That's going to be the length of the segment that we're making from, you know, joint to joint. Uh, let's set that to a length of 15.
So now that that's done, now I can get into sketching. So I'll create a sketch. I'll do it on the, you know, XY plane. And I'll jump right in and create a line. Start from the origin. And actually, as I'm stretching this out now, I can type in "length." And now that's set to be length. So just create a, a vertical line like that with the length of length.
And now I'm going to put the ball on one end, socket on the other. Let's start with a ball. So I have the circle tool. Click at the end there. I'm going to do a diameter of 6 mm. And then on the socket end, the outer diameter is going to be 9 mm. The inner diameter is going to be 5.8. So what that's going to do is if this is 6 mm and it goes into a socket that's 5.8, there's going to be a little bit of interference. So that's going to put a little bit of squeeze on the joint and make it, you know, basically a firm connection rather than something that can flop around. Uh, that interference is also why we can't really do these as print-and-place joints like I know everyone would like.
So with that done, real quick, I'm just going to grab the line tool again. I'm going to extend this one up, extend this one down, just because I know I'll need those lines later. Zooming in on the socket, I need to create basically the opening. So I'll do two more lines here. And I want these lines to be basically symmetrical across this line. So there's actually a constraint for that. I'll go up into the constraints section, pick symmetry, click one, two, and then I want them to be across this line. So now no matter how I edit these, they're always going to be centered on that middle line.
Next, I'll dimension the actual angle between them. So go to Sketch Dimension or hit D. Go between those two. And my magic number for this is 112.5 degrees because that's the first number that I tried and it worked, so I didn't change it. That's three years ago at this point. Okay, so that's basically everything for the socket, everything for the ball.
And now we need the segment that connects them. So we'll go back into the line tool. Start on the socket end, just kind of pick a point, come up and over to the center. And then one more segment for the neck here. Um, just make sure that you don't pick this midpoint here. U, that little triangle means it's the midpoint, so just, just go over a little bit, go up there. We'll set the right dimensions in in a minute. Uh, and now I want those on both sides. So I can go up to the mirror tool. That's in the Create menu. Click one, two, three segments that I want to mirror. And then click mirror line, and that's going to be the middle. Hit OK. And now these again, they're constrained to always be symmetric with each other. You know, doing the mirror command creates that constraint, which is nice.
Uh, going to go back and dimension these now. So the little neck that connects to the ball end, I want that to be 3 mm across. The main segment, I want that to be 5 mm. That can really be whatever you want, but I, I think that five works. And then the length from the center of the ball to basically the end of the neck, we'll make that 4 and a half. And that's because it's going to fit into something that's 9 mm around. Half of that for clearance is 4 and a half, if that makes sense.
So now I think I have everything I need in this sketch. So we'll finish the sketch. Let's start turning this into a solid model. So first, I want to do the ball, the rounded ball. That's a revolve. So I'll click these two profiles. Uh, I don't need to click the ones on the other side, and actually I can't because that would break the tool. So just those two on the one side. And then pick the axis of the center line. Can do that as a full revolve because I want it to go all the way around. That's going to give me the ball at the end and the little neck that attaches to it. I want that to be cylindrical.
Next, what I want to do is bring back that sketch because I'm not done with it. So open the sketch dropdown, click the eyeball, bring that sketch back. Now I want to make kind of the main body of it. So that's going to be an extrude. Click these profiles, not these because that's sort of where the opening for the ball joint is. And then I want this to be going both sides. So I'm going to make this a symmetrical extrude. Um, and then I want it to be 5 millimeters total. But actually, that means I need to pick "whole length" in the measurement because that'll make it be 5 millimeters total rather than 5 millimeters in each direction. So we'll pick "whole length." Make sure this is set to join, so everything is going to join into one body with what's already there. That looks good.
Now I need to do another revolve to cut out the actual socket section. So I'll grab a revolve. I want this profile in here, but it won't let me click it directly because there's a body in the way. So easiest thing to do is just click and hold. That'll bring up this little dropdown, and now I can click profile. That selects that specific profile. That's what I want to revolve. Again, pick axis. I can pick really anything on this center line, and it'll, it'll work. So I'll just pick this one because it's easily accessible. That's going to now cut out that, uh, that socket area.
So I think I have everything I need from this sketch. What do I need to do now? Well, this opening here is a little too small for this neck to actually fit in. So that would limit the range of motion. I want to open that up a little bit. I'm going to do that with the chamfer. So I'm going to go up to the chamfer tool. Come down, click those two. I'm going to chamfer that to 1 mm. Again, all these numbers are just kind of what I've tried over the years and what worked best for me. They're not set in stone. You can experiment, but again, we're just doing what works for me right now.
Uh, what else do I need to do? Well, this is going to be printed on a 3D printer, and it's going to be printed in roughly this orientation. So basically, this face is going to be touching the build plate. But if I look at it from the side, this ball is a problem because it sticks down below what I want to be the bottom of the part. And that sphere is not going to stick in place. So I need to cut off a little bit of this ball. Is the moral of that story? There are a few different ways to do that. What I actually like to do is go up to Modify again and get the split body tool. If that's not up on the toolbar, you can just drop this down again, click split body. So body to split is going to be the only body that I have. And then splitting tools, I'm going to pick this bottom face. Make sure that extend is on and hit OK.
So what this is now done is I can look into the bodies and see, okay, it split into this body and this body. Right, two different parts. Now, that still left this body in place. It didn't actually get rid of it. So now I need to get rid of it. Uh, how do I do that? Well, I could just hide it, but I know I don't need it anymore, so I should probably like actually get rid of it. But if I go over and just hit delete, it's going to warn me. It's going to say, "Hey, if you..." What this basically is saying is, if you delete this, I'm going to forget about it, and anything that relied on it in the past is probably going to break because you've, you've basically just erased it from all of history. And we don't want to erase it from all of history. We want this history here to still work, and that depends on that body actually still existing.
So what we need to do is actually go to this. We can right-click it and hit "remove." So what that did, it got rid of it. It's no longer in that list, right? It's still there, or it's, it's not there, um, but it created an actual feature in the timeline where that thing got taken out. It's now remembering that it did exist, and then I took it out. And I can actually go down and suppress this feature, and it'll come back. So this is really important for parametric modeling where you need a history where it actually remembers what you did in the past in case you want to go back and edit it. Anyway, that's my rant on that.
So this is basically functionally complete, right? You could export this now and 3D print it, and it would work. You'd be able to connect a couple together and be well on your way. Um, there are a few things that I like to do to kind of improve things. First of which is this, this little sharp corner here. I don't really like it. It kind of gets in the way of the range of motion. So I just go ahead and grab a fillet, click that edge and all of the mirrored equivalents of it, fillet that by 1 mm, and that just rounds out that corner and gives me a little bit more range of motion. Don't have to do that, but why not?
Next thing I like to do is I've noticed that when I try and print something like this where it has this cylindrical neck, when this prints, it has to do a little bit of a bridge to get across that, right? And if it's rounded out like this, usually it's going to do like one layer or one line on the first layer, and then on top of that, it's going to do more. And sometimes it just, it just doesn't print all that pretty, you know? It's so tiny that you probably would never notice it, but I'm, I've just noticed that it prints a little bit better when I flatten this out just a little bit.
So to do that, I'm just going to do a quick extrude, which needs a sketch. So I'll pick this plane here, this side plane, and I want this sketch to be basically be attached to this face. So I can do that with a project. So I go into Create, Project, Include, Project. I think this P is the default shortcut for this. It's what I usually use. And I'll just click this cylindrical face and hit OK. And basically, what that did is now that specific feature has been linked to the sketch. And if this feature were to ever move, um, because, you know, I changed that parameter and the length changed, this sketch would come with it. Which is again, a big part of parametric modeling is just making sure that things move where you want them to move if you have to move them.
So to set up the part that we actually want to cut away, I'm going to grab the line tool. Zoom in, come across the bottom, and then just do a little bit offset from that. Dimension between those is just going to be 0.2 mm. It's barely anything, but again, it's just something that I've noticed helps a little bit, so I do it. Finish that sketch, do another extrude. It's already selected that profile again. I want this one to be symmetric, and I can just set the extent type to "all" to make sure that I cut away everything I need to cut away. Hit OK. Now that's flattened out the way I like it. Very nice.
Last thing I'm going to do is what we always love doing in 3D printing, which is just putting chamfers on everything, right? Chamfers, fillets, we, we love just adding extra features to stuff. So I'm just going to do a quick aesthetic fillet on everything, or chamfer actually. Uh, the nice thing about Fusion is that you can pick these lines through the part, right? I can pick that edge without actually flipping it around to see it. That's a nice timesaver. I'm just going to chamfer these by 0.5. That looks pretty nice. That looks like a part. That looks like something I could make an action figure out of. Let's go ahead and save that. We're not ashamed of that.
Oh, hey, what I, you know what I should show you is remember that parameter that we set up? So let me pull that back up. And I use my shortcut to pull that up, but again, that's in Modify, Change Parameters. There we go. So here's my part. Here's my parameter. If I change that, let's say I wanted to be 20, actually. Oh, hey, look, everything updated nicely. I didn't have to go look back, "Oh, I think it's in this sketch," and, uh, "Okay, it's this number. Let me edit that." And no. All I had to do was just change one parameter, and it'll do, it'll update everything because I set it up knowing that that's something that I might update.
I will set up a parameter for anything that I know I might want to tweak later. So a lot of times it is a length. If I want to change proportions on the figure, I'm like, "Oh, I might want his arm to be a little bit longer later," so I'll just set up a parameter for the arm length, and I'll just be able to edit that on the fly later rather than dig back through. Or, you know, width, depth, anything that I think I might want to change later is the moral of that story.
Anyway, this is done. We can export this. We can go put them together. We are now at the part of the video where I ask you to leave a comment letting me know what you want to see in the next tutorial, and I ask you to subscribe so that you can see it, and ring the bell, and leave a like, gift to charity, hug your dad, save the whales, so on and so forth. So go do all that, and I will see you next time. Bye-bye.