- [Instructor] Now it's time to start sketching out
our cut profile.
We're actually going to be cutting away
from the space between our teeth.
We're going to reopen sketch two
and get normal two, smooth this dimension out of the way.
First, we're going to create a simple construction line
that runs up the center of the part.
We're going to use this as a basis
to mirror some other entities.
For the purposes of this lesson,
we're going to simplify the tooth profile
down to a simple three point arc
that's tangent to the center of the part.
In reality, the geometry of the tooth profile
is far more complex and beyond the scope of this lesson.
So we're going to create a three-point arc
that connects the root diameter and the outer diameter
making sure it's curved inward
towards this vertical center line.
And we're going to use the mirror entities command
to mirror the arc above the construction line.
Now, we want it to be tangent
to the center point of the gear.
So we're going to create another construction line here
that runs to the arc.
And then we're going to set the lines
to be tangent to one another.
Okay.
We no longer need our full circles
for our ODI pitch and root diameter.
So I'm going to use the Power trim tool
to just cut away at them to clean up the sketch.
And now we have our basic profile for the space
between the teeth that we're going to cut away from
but we need to fully define the sketch.
Now we have to make sure the pitch point on the tooth edge
is properly defined.
To do this, we're going to create a new construction line
that runs from our center line
to the pitch point of the left-hand arc.
Now, your position on the center line doesn't really matter
because the line is going to be driven by the angle
and its position with this pitch point here.
Now we're going to set the angle here
to be equal to our pressure angle.
We'll set that to be equal to
and select the pressure angle from our global variables.
And we want the construction line to be tangent to our arc
as well as coincident to the pitch point
and our line when inverted there
but we can just simply drag it down to fix that.
Okay.
So now our pitch point for gear tooth
is properly positioned.
The only thing we have to define
is the arc length of the space between our gears.
This will be the arc length distance
between the two teeth at the pitch diameter.
We know that the circular pitch
is equal to PI times the module
and the circular tooth thickness
is equal to the circular pitch,
divided by two, minus any backlash,
in this case, it would be circumferential backlash.
We're going to assume that to be equal to 0.03
times the module.
So the center distance between our teeth
can be derived as the module times PI, divided by two,
plus 0.3, times the module
and that will be our arc length dimension here
for this segment here.
To create an arc length dimension,
we're going to select smart dimension and hold down Control
and select both end points and the actual arc itself.
You'll notice the dimension has a little arc above it
to indicate it's an arc length dimension
and we're going to set up our equation here.
So we're going to do equals our module,
times PI,
close parentheses, divided by two closed parentheses,
plus 0.3, times our module for the backlash.
Hit Okay.
And our sketch is now fully defined.
So we'll exit out of the sketch
and we're going to do an extruded cut
and also to mid-plane
and we will set the direction
to through all in both directions.
That way, if we change the width of the gear,
the cut will still go through the entire part.
And hit okay to create our cut.
We've now successfully completed our tooth cut,
now we just have to pattern it to create our finished gear.