In my high school CAD II class we are 3D modeling radio
controlled cars, 3D printing the parts, and racing them. Everybody is super pumped and things are
going well, but our drivetrain options are somewhat limited. We currently use pulleys press fit to the
output shaft of our motors and rubber bands to transfer power to the rear
wheels, but rubber bands slip badly, break often, and are very inefficient,
wasting a lot of power in the form of friction.
Some students discovered Inventor’s ability to make spur gears with a
true involute tooth profile, and their results were noticeably superior to
rubber bands. We assumed that we could
use that knowledge to make involute bevel gears as well, but Inventor lacked
the “export tooth shape” feature on the bevel gear generator that made accurate spur gears possible. Inventor can generate several types of gears,
but they are all simplified for visualization purposes only, and are nearly
worthless for 3D printing or CNC machining.
Only on the spur gear generator does it have the option to export a true
involute tooth shape, which can be used to make a rapid prototyped, functional
gear. How to transfer the involute shape
of a spur gear into a bevel gear design was a problem that seemed simple at
first, but turned out to be extremely difficult to figure out. With the help of one of my students who was
also taking trigonometry, we were able to come up with a process that generates
working bevel gears using the exported tooth shape from the spur gear
generator.

Here is how we did it.

My 3D printer is an Afinia H480, which I recommend heartily
to all teachers, and I use ABS filament for strength. I have found that the finest functional teeth
that I can reliably print have a module of 1mm.
This means that if the gear has a diameter of 24mm, it will have 24 teeth. Lego gears have a module of 1mm.

Open a new assembly file and save it. Open the Design tab, and click Spur
Gear. Expand all expanders, to the
right, down, and then the” <<” next to the cancel button. In the bottom section change input type to “Number
of Teeth” and size type to “Module”.
Change Design Guide to “Center Distance”. Now you can enter the number of teeth you
want on each of the two gears. A
pressure angle of 20 degrees works fine.
Keep your helix angle at 0. Set
your module to 1mm. It doesn’t matter
what your facewidth is for what we’re doing.
After you have your data entered (Module and Number of Teeth), you can
hit calculate. I’ve never had it tell me
my gears would work. It’s always
“Calculation indicates design failure!”
Ignore this. Click “OK” and
accept the failure again in a pop up box.

Now you should have a couple of gears on your screen. These gears are not ready to be used. If you zoom in you can see that they overlap
with interference. We need to right-click on one of them and choose
“Export Tooth Shape”. We will have to do
the rest of this procedure twice unless your gears have the same tooth count as
each other. Once for the pinion (the
smaller of the two gears) and once for the gear (the larger of the two
gears). Use “Normal” backlash, and
choose the largest value it will let you enter.
For 1mm module gears, it seems to be about .006”. This backlash will keep the gears from
interfering with each other with an imprecise 3D print. Click “OK”.

Now Inventor will take you to an .ipt part, which will be a
cylinder with one of the spaces between the teeth on a sketch on the end
surface. If you were making a spur gear
you would make a cutting extrusion of that space, then do a 3D circular array
of it in the amount of teeth you entered in the gear calculator. We, though, are going to delete the
extrusion, but leave the pinned Sketch1.
Edit that sketch, and delete all of the construction circles. Next do a 2D circular array of the tooth cut,
then trim the outer circle so that the sketch shows the actual gear profile all
the way around. Click “Finish
Sketch”. Now make a new sketch on a
plane perpendicular to that gear sketch.
I use the YZ plane. Draw a
centerline to the right, from the origin, which should be the center of the
gear. Make it pretty long. Now draw a construction line straight down,
from the origin, at least as long as the gear radius and then a little bit
more. Now draw a solid line from the
origin, down and to the right, a little bit longer than the gear radius. The angle between this line and the “down-from-the-origin”
construction line will be 90 minus the inverse tangent (aka arctan) of the gear
ratio divided by two. If I have 32 teeth
on my gear, and 8 teeth on my pinion, my gear ratio is 4. The inverse tangent of 4 is about 76. 90-76=14.
Half of 14 is 7. My angle from
vertical for that line will be 7.

On the Windows calculator, use the “Inv” button to make tan
into inverse tan (tan^-1).

Next, draw a line from the end of that line to the other end
of the centerline. Then, from that end
(end opposite of the origin) draw another line to the angled line sort of close
to the end further from the origin. Make
that line a construction line. It should
look like this:

Next, you will place an angle dimension between the
centerline and the construction line.
This angle will be 90 minus the inverse tangent of your gear ratio,
which in this case will be 14.

At this point you will go back to your assembly file, right
click on the gears, and click “Edit Using Design Accelerator”. This will bring up the spur gear component
generator. Click the notepad in the
upper right corner. This will bring up a
tab in your internet browser which lists the gear parameters. We are interested in Pitch Diameter and
Outside Diameter for the gear we are working on.

Back in the sketch, place a diameter dimension from the
centerline to the lower corner of our triangle, and make the dimension the
Outside Diameter, plus .001”. The
Outside Diameter is rounded in the chart, and if our soon-to-be-revolvoed part
isn’t bigger than the gear sketch that we are going to project on it, it won’t
work, so don’t forget to add that .001”.
Now, for the lower point of the construction line, place a diameter
dimension from the centerline, and make the value the Pitch Diameter. Everything should be purple now, and the
sketch is ready to finish, so click finish sketch.

Our next step is to get a point at the far tip of the cone,
so we need to make an axis through the cone, and place a point at the place the
cone and the axis intersect. Click axis
and click the cone to make an axis, then click the down arrow next to the point
button and choose Intersection of Plane/Surface and Line. Then choose the cone and the new axis, and
there’s your point.

Next click Start 3D sketch (below Start 2D Sketch), then
click Project to Surface. The Faces is
the near side of the cone, and the Curves is the gear sketch. This will project a flat sketch onto the
curve of the near cone. The effect of
this is that the teeth are taller because they are now on the hypotenuse. Without this step the teeth would be too
short when lofted to the point at the far end of the cone. It doesn’t make as much difference on the
small gear, but on the larger gear the difference is significant. Anyway, now we use the loft command to loft
the projected 3D sketch to the point on the far cone. You will use the Cut or Intersect button in
the Loft command to make this happen. I
am not sure why, but one or the other button works, and the other one doesn’t,
but it doesn’t seem to be consistent.
Just try them both and find out which one works. At this point you have a functional bevel
gear, but not a practical one.

You will need to make a plane with a sketch and a cutting
extrusion to cut your gear off at the facewidth you need. Don’t forget to use your Slice Graphics (F7)
button.

Then pop a hole in the gear for your shaft.

The steps are exactly the same for the other gear, but you
need to remember that because the inverse tangent of 4 is 76, on the smaller
gear we used 90-76=14 for our angle. On
the other gear we will be using 76 as our angle. Why is that?
The “pitch cone” of two gears with the same number of teeth will be 45
degrees. No matter what ratio of teeth
they have, the angles of the pitch cones must add up to 90 if the shafts are at
a 90 degree angle. The angled
construction line in the revolved cone sketch was our pitch cone line.

I guess someone has already told you about this but in any case. If you don't want Inventor to tell you that the Calculation indicates design failure you should turn off that Calculation by clicking in the Fx button at the right top corner.

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