The spherical bearing ball will be pretty straightforward to model.
Start by opening up the chapter start file from the course exercise folder
or opening up a new part file,
making sure that the units are set to inch pound seconds.
We'll start by creating a simple sphere and then steadily
cut it down to create our finished product.
So we'll start by making it a new sketch on the front plane
where we'll create a basic
circle centered about the origin.
Then we're going to create a horizontal line
that runs across its equator like so,
and we'll use our trimming tool
to cut away at the bottom half of our circle.
And the last thing we're going to do
is create a center line that runs from the origin horizontally,
like so.
And we'll use a sketch to create a revolve
which will create our initial sphere.
So now we need to dimension our sketch.
So we will set the radius to be equal to our diameter,
which is 1.5 divided by two,
which is equal to 0.75.
Okay.
Now our sketches for defined.
So we'll exit our sketch
and create our revolve bar space
and head okay to create our solid sphere.
Now we want to cut away from our sphere to create our finished part.
The first thing we're going to do is create the two foot interfaces,
which will use the right plane to make a sketch for.
We'll get normal to
and we're going
to create a simple center point box centered at the origin
like so.
And we want the
top and bottom lines of the box to be tangent to our sphere.
So we will select the line and hold control and select the edge of our sphere
and select tangent for the relation.
So now we just need to define
the width of our box here.
We'll create a new dimension
and we'll set the width
to be equal to one inch.
So now we have a fully defined sketch
and we can cut away from these two outside areas
here and here,
and we'll do an extruded cut
and we'll just select
through all both directions.
Now it wants us to cut away the area encompassed
by the profile that we just sketched, which we don't want to do.
We actually want to click on this flip side cut here.
So they'll cut away at these two areas of our solid body
that are not encompassed by the sketch of our rectangle
hit. Okay.
And now we have our two flat faces.
All right.
Our next step will be to create our four diameter,
which is just a through hole that runs from one phase to the other.
We do this in a few different ways,
but let's make a new sketch on the front plane.
We'll get normal to.
And we're going to create a
another center point circle
like so.
And this one will dimension
to be one inch in diameter
and exit our sketch,
and we'll do a new extruded cut
for the direction we'll go through all in
both directions
and hit.
Okay.
And now we have our board diameter.
The last thing we're going to do is add
a simple chamfer to these two corners here and here.
So we will select chamfer
for the depth.
We'll set it to be equal to 0.01 inches,
and the angle will keep at 45 degrees.
And we just select the bore diameter,
which will automatically select both of its edges and hit.
Okay.
Now, for our material,
we're going to set it to be equal to a S.I.
three or four stainless.
But we want to change
the appearance of our o.D
because in reality,
these balls would have a dry film coating
which would give them a darker, almost graphite like appearance.
So we're going to try and replicate that.
So to set the appearance of just a single
surface on a part,
we just have to highlight the surface and go up here to appearances
and we're going to
click on this face one here.
Now, the closest thing I can find to
the graphite texture is sandblasted iron.
So we're going to expand our metal folder
and then expand our iron and we'll select sandblasted
iron here
and hit.
Okay.
Now, if we turn on the Real View graphics
and okay,
we can see this nice texture that's there.
So if we were to do any 3D renderings,
the ball would look very realistic to the finished product.
So we'll turn off our real view graphics.
Our spherical ball is now complete and we're ready
to start working on our assembly.