- [Instructor] Now that our gear plank is complete,
we're ready to start to create our gear tooth cut.
Our first step will be to sketch out our pitch root
and outer diameters.
So I'm going to open up a new sketch in the front plane.
Set the view normal two.
And create two concentric circles based
about the parts origin.
They will be for the pitch diameter and our root diameter.
We are also going to need the outer diameter
for this tooth cut.
So we're going to select convert entities
and click the outer edge to capture that.
Now we need to fully define our sketch
by defining our pitch diameter and root diameter.
So we're going to open up a new dimension
or a pitch diameter and enter in our pitch diameter equation
which is equal to our number of teeth
times our module.
Hit the green check box to create the equation.
I'm going to set the pitch diameter circle
as a construction line because we're only going to use it
as a reference when we create our gear tooth cut.
Our second equation will be for our tooth dept,
which is a bit more complicated.
This is going to be the distance between the outer diameter
and the root diameter.
Since the equation varies based on the module value,
we're going to set up a basic if statement.
So SolidWorks knows which equation to use.
To review, we know that the tooth depth is equal to 2.4
times the module
if the module is less than 1.25.
And is equal to 2.25 times the module,
if it is greater than 1.25.
Since the equation is more complex,
we're going to create a new global variable
for the tooth dept.
So go to tools, equations
and for the variable name we're going to enter in
tooth dept and we're going to create our basic if statement.
So if, open parentheses our module
is less than 1.25.
It is 2.4 times our module.
Else it is 2.25 times our module
and close parentheses.
Now we can test this because we know our module
is actually one.
So if it is less than 1.25,
which it is we use this equation.
So it's basically 2.4 times the module.
So 2.4 times one, which gives us 2.4.
It's always good to do a quick check by hand
to make sure that SolidWorks
is giving us the correct values.
We don't have any type of graphical errors in our equations.
Now there are tooth depth is set up.
We'll hit okay to close out the equation window.
And we have to go back into our sketch here.
Now we need to create a dimension between our outer diameter
and our root diameter for the tooth depth.
To create this dimension,
I'm going to select smart dimension
and hold down control while clicking
the outer diameter and the root diameter.
This will create a dimension for the distance
between the two circles.
And we are simply going to set this to be equal
to our tooth depth global variable.
And hit okay.
Right.
Now our sketches fully defined, we'll exit out.
Now that our ODI pitch and root diameter sketch
is fully defined,
we're ready to start to create our tooth cut.