- [Instructor] Let's talk about mates inside of SolidWorks.
Now that I've got my assembly started,
I've got individual parts inside of my assembly,
I can grab and I can move these components
around on my screen
by left-clicking on 'em and dragging 'em around.
I can rotate them by right
mouse clicking on 'em and rotating 'em around.
Now we need to actually connect them together using mates.
So the best way to mate something together
is to actually say what you would like
to connect together out loud.
It might sound a little funny to do
but if you actually say it out loud,
it really makes it easy to figure out
what things we need to click and mate together.
So before we do that,
let's click on the Mate toolbar right up here.
So click on Mate,
and notice we've got all these standard mates.
We get Coincident, Parallel, Perpendicular,
Tangent, Concentric, and so on.
Now SolidWorks are actually figure this out for us.
If we choose nothing over here in this window,
if we just start selecting faces on our parts,
SolidWorks are generally
come up with a suggested mate type.
Now we can change that,
but let me give you an example of how it works.
So if I choose this face right here,
I say I want to connect that face.
and I rotate my entire assembly around here,
and right over here, I want to select this face here.
So I'm saying out loud is I want to connect this face
to that face, right?
And as soon as I do, notice the two slide together.
So notice from the side, those are touching
but it is too low, right?
But we have to add generally three mates
to each individual part to fully define
where it is in space.
When that looks okay, click on the green check mark
and now we've added our first mate.
So check this out,
I can slide this part around
but it will not come off of that face.
If I try to click on it, it just won't come off.
It looks like it's coming off here, but it's really not.
It's actually way out here in space.
So you got to be careful with that.
So make sure that you know where your part is.
So again, that's touching.
Now we want to add one more mate.
So I'm going to choose this face here
and then the end face here.
So notice those slide together.
Now I can still move this up and down
but I can't move it right to left, it won't go.
It can only go up and down
because it's attached to the face
and now these two faces are attached together
if I exit out of the Mate command.
Over here, I have a little folder called Mates.
And if we twirl down,
you can see I've got my original mate here,
I've got this mate here and I've got this mate here.
So this mate here,
this coincident mate actually happens to be for this block.
The very first block here
and the mates side there is that coincident,
which is tying that together.
So the mates that are attached
to just this little purple wedge here,
if you click on that part itself, you can see here it is.
And you can see inside there, we have a Mate folder
and those two mates are attached to that block.
So you can grab or find those mates
in the FeatureManager both ways.
One, if you click on the part itself,
you can see which mates are attached to it
or down here are all the individual mates in this assembly.
So you can get the exact same mate two different places.
Now we want to add one more mate.
So if I come over here, I'm going to say,
"Hey, I like to have this face down here,
attached over here."
But if I get a little closer, I notice a problem.
Look, these are not at the same angle.
So if I try to make that face touch that face,
it's going to cause an issue
because SolidWorks cannot solve that type of mate.
We've already defined this face and this face are touching.
So let's see what SolidWorks does.
I'm going to go ahead and try to create a mate,
I'm going to choose this face here,
and then I'm going to come down here
and I'm going to choose that face there.
And then I'm going to say, "Okay, yeah, do it."
And it's going to say,
"Well, I can't automatically select a mate for you
'cause I don't know what you want me to do."
So you're saying, "Hey, how about coincident?
Let's do that."
Click Okay, and it's saying,
"Hey, you can't really do this, right?"
It's saying add this mate to break other mates
or add this mate to over define the assembly.
It's asking you how to resolve the situation.
So I'm going to go ahead and just add this mate
to over define the assembly and then get out of this.
Now notice what happens.
I get all these yellow and red marks
all over my FeatureManager to just, it's a scene,
I don't know what's going on here.
And it's saying, "Hey, I don't know
how to solve this for you".
So it's saying this part or this assembly down here,
this mate in this assembly is causing us an issue
and here's the troublemaker.
And it's also affecting this mate over here.
So I can delete either one of those to solve the issue.
So if I delete this one here,
hit Delete on my keyboard, say Yes,
then this mate over here says, "Okay, I'm okay."
It automatically rotates the part around
when you click on it.
So now these two things are connected together,
just like they were.
And over here you can see that this angle is different.
And so we've actually deleted that mate
that was causing the issue.
So you could delete either one of those.
Now if you wanted to find this a little further,
we can come back to the Mate command.
And instead of choosing a face to face,
I could choose like a face to maybe this line.
And notice that line comes over and now hits that face,
and everything's okay
because SolidWorks can now solve this issue.
Now I want to spin around and do a couple extra mates here.
How about this one over here?
I could say the inside of this circle here
or this washer to the outside of that.
Notice those two things slide together.
Now I can move this in or out,
but it's not fully touched or it's not fully defined.
If I choose this face here, touch this face here as well,
now those two things mate together.
Now is this fully defined?
Is there three mates?
No, there's only two.
So the degree of freedom
that's not been defined is rotation.
I can rotate this around.
It's really hard to see
because it all looks exactly the same,
but that part only has two mates.
So it's not a 100% defined.
But what I can do is, if I come over here,
I can click on the part and see where it shows up.
Here's my part.
And notice that little minus sign right there.
If you see a minus sign, that means it's not fully defined.
It's undefined or are not fully controlled.
So if I were to go back and add another mate,
like maybe like the right plane to the right plane.
I could say, add a mate between those two things.
Then all of a sudden that part becomes fully defined.
Notice over here, that little minus sign went away
because now I defined it in all three mates.
I've controlled it.
So it's connected to that circle
over that pin and it's touching that face.
And now you have a fully defined
part inside of of your SolidWorks assembly.