- [Instructor] So far, we've learned about linear patterns,
but in this movie,
we're going to focus in on circular patterns.
Now, before we can create a circular pattern,
we actually need to create an assembly.
So, I'm going to go ahead and take this part right here
and create an assembly from it.
So, I'm going to head up here to file,
and make assembly from part.
And go ahead and include that one in, click Okay,
and there is my first part in the assembly.
Now, let's go ahead and add in one more component.
So, I'm going to go over here and say, open.
And in that same folder, is this socket head cap screw,
go ahead and open that up,
and let's go ahead and take that one there.
I'm going to tile horizontally,
and I'm going to just go ahead and drag and drop this.
So, here's the component here.
Here's the assembly that's going to drag it into the assembly
and bring it down.
Okay, now, let's do our very first mate.
So, I'm going to spin that component around
by holding down the right mouse button,
then come over here and click on mate,
and I'm going to choose this hole right here,
and the outside of that screw.
And then bring it up a little higher,
choose this face right down here,
spin the entire model around
holding down the middle mouse button
and then grab that bottom face.
Okay, so, now we've made it together
our very first component here.
Click on Okay.
Now, instead of adding in manually
all of those other socket head cap screws,
that'd be a lot of work.
How about we just do a circular pattern?
So, under the linear component pattern,
click on the dropdown
and you can see we have a circular component pattern,
click on that.
As far as the direction, what do I want to rotate around?
Now, I could choose something like the outside surface here
and that'll work, or you could choose the center axis
by turning on temporary axis directly under here,
and come over here into temporary axis,
and now you can see that center axis.
Couple different ways you can do that.
Okay, now, the component I'd like to pattern,
notice this one here,
I'm going to go ahead and choose that screw
and then define what angle I'd like here.
So, I know the angle is 22.5 degrees
between each one of these.
And notice, as soon as I just click
on this little up arrow here,
I can add all those screws all the way around,
just that easily.
Or you could switch to equal spacing
which will do exactly the same thing,
but if you do that, notice the screws do pattern around
a little bit differently.
So, keep in mind if you want equal spacing
or you just want to type in the value here
as far as how many screws you want.
If you want to skip an instance,
you can click into this box here,
and then click on any one of these pink or purple dots,
and you can say, skip.
Click on this guy over here, skip
or you can even modify it if you wanted to.
So, a couple different options there,
but that's how you can easily skip those instances,
and then the values are right over here.
And if you want to bring one of those back,
just click on this box, hit delete,
and then that will come back.
So, anyways, that is how you use the circle pattern tool
inside of SolidWorks.