Learn how to mate parts into an assembly.
- [Instructor] In this movie, we're going to be learning how to create assembly mates. Now, what a mate is is a way to attach two components together. Generally, each component will need about three mates to fully define where that component is in space. Now, your very first part you bring into assembly more than likely is going to be fixed. So I click on this item right here, try to move it around, and nothing happens. If you look over here, you can see that this is the first item, and more than likely, if you right-click on it, you can come over here and it says either Fix or Float.
So if you fix it, it can't move, and if you right click on it again, you can say Float, and that'll allow you to move it around. Now the other option is if it's already been mated to something, like a coincident mate, that will lock it into the origin, and it won't be able to move, so it's either mated completely, or it's being fixed if it doesn't move on your screen. So, more than likely, you want to do it to the first part in our assembly, and then we want to bring all the other components to that one part. All right, so the next thing we want to do is we want to enable the Mate command, and it's under the Assembly toolbar, right up here under Mate.
Click on that one there, and you can see we've got a whole bunch of different styles of mates, and these are just your standard mates, but if you go down a little further, we also have Advanced Mates, and we've got a whole list of advanced mates here. You can take a look through, as well as some of these mechanical mates. So, under Mechanical Mates, you got all these over here as well. We don't have time to get into every single one of these things, so let's just go ahead and focus on the standard mates. So, Coincident means two things are touching. Parallel, obviously, means they're parallel. Perpendicular means they're perpendicular. Tangent means if it's got a curve, it's going to be tangent to another flat object or another curved object.
Concentric means that you have, obviously, a circle that's inside of another circle, and they're concentric to each other. And I'm going to show you how to do those things right now. All right, so the first mate we're going to do is this wedge. So I want to take this back surface here of this block, and notice the block does change colors as I do select that, and I want to mate that together with this back surface over here. Now, watch what happens as soon as I click on this surface. It slides over here in place, and you can see now, that these are actually aligned. So, if I zoom in there, you can see these are aligned, because I've mated them together.
Now, is it fully defined? Absolutely not, but it does have a plane made between those two faces, so those are now touching. All right, click on the green check mark, and then we can continue to mate these together. How about the end of this block here, with the end of this block over here? Notice as soon as you do that, the two components slide together, and now we've added two mates to this one block. Now if you get out of this tool here, if we just close it out, or click on the reject mark, either way, you can then move these components around. And notice it slides up and down, but you can't slide it left to right, because we've already defined its mate over here.
I also can't pull that block out, because I fully defined it. Now, sometimes, you want something like this. You want it to be able to slide around. You don't want it to be fully locked into place, and that's okay. But in this case here, we probably want to define it a little bit better. Now, I do want to point out that up here, these angles are not exact. Up here, you can see here there's a little bit of a gap here, and it's a little tighter over here than it is over here, and therefore, we can't do something like a coincident mate, because it would fail. That would cause some kind of an issue, because I can't make these two planes touch, because this one's already been defined over here.
So, whenever you're selecting a mate, you have to choose a mate that will actually work for the circumstances you're in. Now, for instance, I could choose something like a line. I could say, "Hey, this line over here," and I can make that coincident to, maybe, this plane over here, or this other line here, and that would work, right? Because it's not violating any of the other mates. Now, if you do try and add a mate that would cause trouble for another one, you're going to start getting some errors. So, let's go ahead and try and do that. Go to a mate, let's go ahead and say this surface here, and the surface over here, and let's go and make them coincident, and click on OK.
And it says, "Hey! Adding this mate is going to break other mates. "So, do we want to do that? Yes or no?" So, add this mate, uh-oh. And it gave you all these issues and errors. This is over-defined, and we've added that mate even though it's going to mess up the other mates. However, don't worry. We've replaced that mate now. We've actually broken this other mate, and everything's okay, because, it works, but you can see here our, the issues. So here's this other mate. It's saying that it can't be moved into position that makes it satisfied.
Same thing over here. These ones here are the ones that are actually, probably, causing the issues, or which are in violation. So, if you were to delete this mate right here, click OK, now everything goes back to being happy. SolidWorks knows how to solve this. Is the mating scheme correct, as far as the model? Probably not. We don't really want to have it going in this direction here, but as far SolidWorks is concerned, it is happy with the mating situation as it is right now. You might want to modify that later on, but for right now, let's just go ahead and leave that where that is. Now, I do want to point out, because we deleted that other mate, now we can actually grab this block and slide it this direction, so that's causing us another issue that we need to come back for.
But we can easily resolve that by choosing something like a mate, and we can say something like, this top edge here, and maybe that surface there. And those will slide together, click on OK, and now we've fully defined those mates. All right. Next one's going to be a concentric mate, so how about we choose the outside surface here, and maybe the inside surface over there, and those two objects just automatically slide together. Now, SolidWorks, generally, will choose the correct mate for us. If you choose two cylinders, it's automatically going to choose that concentric mate. If you want to change that to something else, you can.
So if you want to say, "Hey, instead of being concentric, "I'd like to make these tangent to each other." And that does modify that mate, and now we have a tangency relationship between the two. So, a little bit different here, but it does allow you to kind of move things around. Now, if you accidentally chose the wrong mate, you can always just close out of the Mate command, and come down here to that Mate tab, make sure you twirl it down, and you can see all the individual mates. If you don't like one, click on that mate, hit Delete on your keyboard, and just remove that mate. All right, let's go back and edit correctly this item.
Let's say, I want to go from the outside of that to the inside of this. Concentric, click OK, and we're looking good. Now maybe this surface here, mated together with this back surface here, it'll slide together, and we're all set. The last one's going to be this little peg. And if I choose something like this surface here, I can mate that to that surface there, and everything just slides together. So in that case, you only really needed the one mate to fully define where that is, because I chose two conical style surfaces that automatically meshed together, and it's going to fully define where that is.
Now, I do want to point out that this part still can spin around its axis, but in this case, it doesn't really matter. So that's how you add standard mates to your parts. You can see there's a lot that goes into mating, and there's quite a bit of tools available to us. You really just have to think through how you want to attach these components together, in the best and most robust way to do so.
First, see how to how to use the sketch tools to create two-dimensional sketches that become the foundation for 3D objects. Next, look at extruding and revolving 3D features; creating complex objects using the Sweep, Loft, and Surface tools; and modifying parts. Learn how to create uniform holes with the Hole Wizard, and explore more advanced modeling techniques using equations, mirroring, and pattern tools. Then review best practices for putting parts together in assemblies and building robust structures. The course wraps up tips for creating detailed drawings that relate the final parts and assemblies to a manufacturer, complete with an itemized bill of materials and drawing notes.
- Working with templates
- Creating sketches
- Extruding and revolving features
- Applying materials
- Sketching lines, shapes, and polygons
- Trimming, extending, and transforming geometry
- Adding fillets and chamfers
- Working with planes and coordinates
- Creating patterns
- Modeling advanced parts
- Making holes
- Designing with blocks
- Building assemblies
- Mating parts
- Linking sketches
- Using design tables
- Creating part and assembly drawings
- Creating dimensions
- Adding annotations