From the course: SOLIDWORKS 2022 Essential Training

Creating component Mates - SOLIDWORKS Tutorial

From the course: SOLIDWORKS 2022 Essential Training

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Creating component Mates

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- At this point in the course, we're going to dive in a little deeper into the assembly environment, and start using the mate command to connect to these components together. Now, I do want to point out before we get started that the first component in this assembly is this one right here and notice the little F in the front of its name. That means that one is fixed. So, everybody is going to be mated to him. Looking from the side can see these components are just kind of free floating around here. And we probably would like to get them all on the same plane. To do so, let's go up to the mate command. Now we've already looked at the coincident mate a little bit, but I do want to point out this little button right here called multi mate mode or multiple mate mode, click on that one there. And that will allow me to choose one common mate face, and then I can choose other mated items. Just click on them here and here. So I got three of those things and then click on 'Okay'. And I've added three mates very quickly. Instead of using that mode, I could actually add three individual coincident mates but it just makes a little bit quicker to do'em all in the one mate command. Okay. Exit out that or click on the green check mark. And now under the mate command, you can see I've got those three different mates that have been added. And I can still move these components around. They all just happen to be on that same plane at the top. Okay. Now, let's jump into mate again, and now we've done the coincident mate. How about parallel mates? Click on parallel first and let's choose a couple components to be parallel. So, I'd like this component here and this component there to be parallel. There they are. All right, so I can't rotate. I can grab it and try to rotate it around, it won't rotate. I can get closer or further away but I can't rotate the component anymore. These components over here, I can still rotate however I'd like. How about perpendicular? Click on perpendicular Choose this phase here and that phase there. And now those components are perpendicular. You still need a couple other mates to define where it is in space, but it will always be perpendicular to this one fixed phase right over here. All right. How about the tangent mate? Click on tangent. And I'm going to choose that phase right there and choose one of these little cylinders. Notice right there it's tangent. I can also switch it to the other side if I'd like. Click on 'Okay' and now that's going to just slide along there. The other thing I'd like to do is make the top of that and the top of that coincident, so, I can see the sliding in action a little bit easier. So there it is. Okay. How about concentric? Choose concentric. I'm going to choose the outside of this cylinder and the outside of that cylinder. And those are going to slide together. Now, I've got one of those, it's still free floating, a little bit higher than the other one. And I can define that a couple different ways. Ones that I could actually add a distance here or I could just lock'em in space. If something like this looks good and I just want to like freely place it there, what I can do is I can choose this component here, this component down here, and then just choose lock. So, I'm locking them together. And now they just float and slide together without actually having any hard number defining a space between the two. And they don't necessarily have to be concentric either. It could be anywhere in space and just lock two items together. And that works really well. All right. Couple other things we want to look at down here are the distance. Click on distance and then define a value. So, maybe from this phase here to this phase here, I would like to define a distance of maybe like three inches. Okay. Type that in. And now that is defined as three inches forever. It's also parallel, if you remember from what we did earlier. So, that has two mates controlling where that is. We can still slide this left to right. And if you want to lock that down a little bit more we could just choose like the end of this and the end of that, those we coincidence, And now this part is fully controlled, and notice over here, If I click on it that the little minus sign in the front is gone. Right now that is a fully defined part. This one is fixed. And then everybody else's still has a little minus sign in the front, meaning it is got some degrees of freedom to move around. All right, back over here to mate. The last one we got to look at is the angle. Okay. This component here still has the ability to rotate around. So, the first thing I want to do is I want to create a hinge. So, I'm going to choose this edge here and I'm going to choose that edge there. Those are going to slide together. And now I've got this little hinge that opens up, and then I can define an angle by choosing like this face right here, spin this around that face over there, and choose the angle, and type in something like 30 degrees. And now we've defined that angle. Click on the green check mark. And now under the mates folder here we can see we've got all those individual mates. If any one of those mates you don't like, you can of course just click on it, hit delete on your keyboard to get rid of it. Or you could actually edit the feature. You can change to a different style of mate by getting in and modifying that mate feature. Bunch of cool things you can do there. So, hopefully this gives you a broad overview of the major mate tools we're going to be using to assemble our components together, in the assembly environment of SolidWorks.

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