In this video, learn how to generate a simplified model of the base of a robot.
- [Instructor] So let's start off by designing the base for our robotic arm. So I'll start by creating a new sketch and I'm going to choose the top plane, in this case. From here, I'll just draw a center rectangle. Going to start from the origin point here and throw on some dimensions, maybe 180 by 180. Notice here, I'm using millimeters. Of course, you can use inches, if you'd like, and I'm really just kind of making up these dimensions so you can throw in whatever dimensions you may like for your designs, if you'd like to follow along with me here. And then really, I can finish off that first sketch, and now I can extrude this out a little bit. So I'll extrude this maybe 10 millimeters or so, and say okay. So from here, now maybe I'll create a new sketch on my top face here. So again, create a new sketch. In this case, I won't select a plane, but I'll select my top face of my first extrusion here. And then maybe just sketch a circle. Again, starting from that origin point and I'll throw in a dimension about 140 millimeters or so. That should be a finished sketch there, so I can stop that sketch. And again, extrude that out a little bit. Extrude again, grab the profile there, and I'll extrude this maybe 100 millimeters or so there. Say okay. And now from here, I might create another new sketch. I'll create a new sketch and I'm going to create it on the front plane, in this case. Grab another center rectangle and place it just about here, so and I'll again, throw in dimensions maybe about 40 by 80. Okay, so I have the size of my rectangle here, and now I want to also throw in a dimension offset from the origin, let's see. So I'll throw in a dimension here, and offset this from the origin, let's say about 60 millimeters, and now that's coming in fully defined or fully constrained so that's looking good. I can finish that sketch off, as well. And extrude that sketch out, so let's do one more extrude here, grab my sketch profile, and this one, let's try extruding it out maybe 100 millimeters or so. Now notice in this case, by default, it looks like it's doing a cut here so I can confirm that in my options. The default operation is set to be cut. Of course, I'm not looking for a cutout here so I can change that, of course, to let's say join, and now that's looking a little bit better to me so I can say okay. And now I more or less have the general shape of my robotic base. Let's do one cutout here on the top face here, so again, I'll create a new sketch. In this case, I can draw a circle, or I make use of the offset tool so I'm going to offset, let's say, from this outer edge here and offset about five millimeters, sorry, and I'm also going to flip the direction. Right now, it's offsetting outside of my extrusion. I want it actually inside of my extrusion, something like that, and I can say okay there. And again, that sketch is looking good to me so I can stop that sketch. Let's do a cut of this profile, and let's cut that down three millimeters or so. Okay, so that's looking good and the operation is set to cut so that looks okay. I can say okay to finish that off and that's looking good to me here. So in the final step, maybe add some fillets at the end, but maybe I want to add some holes in here, as well, so mounting holes so I can mount this down to the ground or whatever it may be. So I can input holes one at a time, which is fine, but let's say I wanted to throw in four of the same counterbored holes. I can do that all in one step, as well. I'll just have to sketch out the sketch points for the locations of my holes first. So let's create one more new sketch here, so create a new sketch. I am going to choose this top face here. And then what I can do is just set really the location point. So I can sketch some points here. And this is going to be essentially where the center point of my hole would be, since there may be a point here, point here, point here, and a point here. And then of course, I can throw in dimensions and constraints there to finish that off and I'm just going to say all of these will be about 10 millimeters from either edge here. So throw in all of those dimensions here quickly. Of course, you could use relations and constraints here, as well. I'm just going to throw in dimensions here quickly. This should be 10 millimeters from each edge and now that's looking good so I can finish off that sketch. And why that's useful is now I can create some holes so I'm going to use the hole command here, but instead of just a single hole at a time, I can now use placement from sketch and I can select all the sketch point I'd like, so in this case, each of these sketch points. Okay, and if I'd like, now it's creating four holes here. I can zoom in a bit and see, you know, what exactly my hole's going to look like so this is a counterbore hole. That's looking pretty good here, but I can define any parameters I'd like here. So the outer diameter of my counterbore here, maybe I want 10, maybe I want 12, whatever it might be. 12 here, let's say. How deep my counterbore may be, the angle, and then my inside diameter here, as well, six. And again, you can just customize and define these parameters to be whatever you'd like to fit your exact counterbore hole it needs, in this case, but and I can say okay. And notice that I have to create this custom hole for all four holes, in this case, by using sketch. So now I'm looking pretty good here. I'm going to just finish it off with some fillets there, so I could throw in a few fillets here. It's got maybe the outer edges first. And maybe these outer edges as well. 'Kay, and then throw in a fillet value, let's say, let's try about 10 millimeters there or so, and that looks okay to me and then maybe just a few other fillets just to finish it off. Inner edges, perhaps, here, and this outer edge here and throw in a smaller fillet radius of I think about two millimeters there and say okay. And now we kind of have a simplified design of our robotic base component here.
- Designing the base component
- Designing links
- Using the plastics and casting design tools
- Creating a mechatronics assembly
- Routing wire
- Creating the final outputs