This is how to make a 40-tooth gear. The gear diameter will be
calculated automatically based on the constraints that we set. With
40 teeth, the tooth spacing will be 360o/40 =
9o. We'll start by drawing half a tooth, then mirroring
it to make a whole tooth, and then copying that feature 40 times.
Start SolidWorks and begin a new part. Set your units to IPS.
Begin an Extruded Base feature on the Front Plane.
Make a circle centered on the origin with a rough radius of 0.8
inches (diameter 1.6 inches). Don't set a hard dimension. Make the
circle "for construction" (check the "For construction" box in the
Draw a roughly 1 inch vertical construction line from the origin
straight up. Make another roughly 1 inch construction line, also
emanating from the origin, but angled slightly to the left of the
vertical line. Then use the dimension tool to set the precise angle
between the two construction lines to half the inter-tooth angle, or
Create a point where the vertical line intersects the circle.
Draw a short horizontal line beginning somewhere on the vertical
line outside the circle, running to the left. Dimension the length of
this horizontal line to 0.0085 inches. (Set the dimension to display
4 digits of precision instead of the default 2 digits.) Dimension the
distance between the right endpoint of the line and the point you made
on the circle, which should be directly below it, to 0.04 inches.
Draw a new line beginning at the left endpoint of your horizontal
line and moving diagonally down to the left, terminating on the circle about
half-way between the two construction lines. Dimension the angle between
this line and the vertical construction line to 30o.
Draw a centerpoint arc, centered on the origin (point 1). Point
2 should be the left edge of your 30o line. Point 3 should
be on the circle but well to the left of the left construction line.
The arc tool doesn't want to make really short arcs, so we'll draw the
arc longer than it needs to be, and afterwards move the left endpoint
to the correct position.
Click and drag on the left endpoint of your arc and snap it to
the left construction line. Note: centerpoint arcs don't always snap
to the place you want them to. Instead they may create a spurious new
point that causes problems later, so always check the endpoints after
creating one of these arcs. To check an endpoint, click on it, wait
for the pop-up menu, then click on the "Select Other" icon. If you
see more than one Point in the pop-up list of objects, you will need
to merge the points. To do this, click on the first point in
the pop-up list. Then shift-click on the point itself (not the pop-up
list entry). This should leave you in the properties editor with two
points selected; click on the Merge relation to merge them. Check the
other endpoint of the arc as well.
Dimension the arc length to 0.0085 inches. Note: to dimension the
true arc length instead of the straight-line distance between the
endpoints, first click on each endpoint, then click on the arc itself.
You'll see a curved line appear above the dimension value. If you
can't get this to work, just dimension the linear distance between the
endpoints; that's close enough. Set the dimension display to three
digits of precision.
All your lines should now be black (fully defined), and the display
should look like this (click on the image for a larger version):
Click on "Mirror Entities" and select the arc, the 30o
line, and the horizontal line as the entities to mirror. Then select
the vertical construction line as the line to mirror about. Click on the
green checkmark to complete the mirroring.
We need to make a closed shape in order for the extrude to
succeed. So draw a centerpoint arc whose center is the point you
created on the vertical construction line, and whose endpoints are the
left and right edges of the respective arc segments. Remember to
check the arc endpoints and merge any duplicate point objects. The
display should now look like this:
Accept the sketch and set the boss-extrude depth to 1/8 in. You
should now have one gear tooth floating in space:
Now we're going to make the body of the gear. Begin a new
Extruded Boss/Base feature, again sketching on the Front Plane.
Make a circle centered on the origin with a radius of roughly
Select the circle, and then shift-click on the tiny little arc
edge at the left base of the gear tooth. This should leave you in the
properties editor with an arc and an edge selected.
Add a Tangent relation to make the circle coincide with the edge
Accept the sketch and set the boss-extrude depth to 1/8 in. You
should now have a disk with one tooth on it:
On the Features tab, select Fillet and add a 0.0125 inch (not the
default 0.1 inch) radius fillet to the four edges of the tooth:
On the Features tab, click on the Linear Pattern pulldown menu
and select Circular Pattern. In the Parameters box, select the
circular edge (not the flat face) of the disk. Check the Equal
Spacing box, then set the number of copies to 40. At the bottom under
Options, check the "Geometry pattern" box. In the Features to Pattern
box, select the first Boss-Extrude and the Fillet feature.
(You will need to open the features tree to select these features.)
You should see a yellow outline of the 20 teeth. Click on the green
checkmark to accept the pattern.
Finally we want to make some holes in the disk to stick a pen in.
The holes should be at varying distances from the center in order to
produce different spirograph patterns. Begin by creating an Extruded
Cut feature on the surface of the gear.
Draw some circles of diameter 0.1 inches (radius 0.05 inches) at
various distances from the center. You can make all the circles lie
on a line, or you can arrange them to form a spiral or some other
pleasing pattern. The final result should look like this:
Make Some More Gears
Make two more small gears with different numbers of teeth, somewhere
between 30 and 60. Remember that the inter-tooth angle is 360/N where
N is the number of teeth; in your sketch you will use half this angle
for the construction line. SolidWorks will automatically calculate
the gear diameter based on the sketch relations you've defined. You
will also need to specify the same value of N in the Circular Pattern
feature. Note: sometimes changing the number of repetitions in a
Circular Pattern causes rebuild errors. In that case, simply delete
or suppress the feature and make a new one.
To make the outer ring of the spirograph, construct a gear with 123
teeth. (Is it significant that this is a prime number?) When we cut
out that gear, the plastic that remains can serve as the outer ring
for the smaller gears you made. We'll draw a circle around this ring
in the next step.
Make a Drawing
Do File New and create a new Drawing (not Part or Assembly) document.
Make sure the units (bottom left corner of the screen) are IPS
(inches/pounds/seconds) and not MMGS or Custom.
Set the sheet size to "custom" and enter 12 inches by 12 inches as the
width and height, then click "OK".
Insert a part onto your drawing. Remember to hit Escape to cancel
insertion of additional views of the part. In the properties manager,
set the part to use sheet scaling, not custom scaling.
If your part has circular holes that show up with centerlines (cross
shapes) in the drawing, click on and delete the centerlines.
In the Feature Manager Tree, right click on Sheet1 and select
Properties. Verify that the sheet scaling is 1:1; somtimes it
defaults to 2:1.
Lay out all your gears on this one sheet. The ring gear should be a little
under 3.25 inches in diameter. If it's 6.5 inches, the scaling is wrong.
To make the outer edge of the big ring gear, switch to the Sketch tab
and draw a circle enclosing the 123-tooth gear. This circle will
become another cut line; we'll throw the 123-tooth spur gear away and
keep the ring gear that surrounds it. Add four tiny holes (0.060 inch
diameter) around the edge of the ring gear so that we can thumb-tack
it in place while making spirograph pictures.
To save plastic, you can nest one of your other gears inside the ring
gear, since we won't be keeping the big gear, only the ring.
Save your file as a SolidWorks drawing file. This is important in
case you want to go back and edit any of the individual parts; the
drawing file will automatically update, but a DXF file will not.
Make a DXF File
Once you've created your drawing file, choose "Save As" and save the
file again as a DXF file.
Run Inkscape, set the file type to DXF (it always defaults to DWG),
and open the DXF file. Zoom out and you may see a "SolidWorks
Educational Edition" banner in the bottom left corner. Click on the
banner lines and hit Delete to remove them. (If running on a MacBook
you will need to press function-Delete.) Then type control-A to
select everything, and set the color to blue.
Hit Escape to deselect everything. Then click and drag to select any
internal shapes that should be cut first (such as the little holes in
your gears), and set their color to red. If nesting one gear inside
another, choose another color, such as green, for that. The idea is
to be able to cut shapes from the innermost outward, because when a
piece of plastic is separated from the sheet it can drop slightly and
thus fall out of alignment with the laser.
Select "Save As" in InkScape and set the file type to "Desktop Cutting
Plotter (AutoCAD DXF R14)". Click "Save", then set the base units to
"mm" and click "OK".
Cut Your Plastic
Remove the paper backing from your acrylic sheet before cutting.
Otherwise the laser will burn the paper and leave burn marks on the
Follow the Rabbit Laser
For 1/8 inch acrylic the recommended power setting for the Rabbit
Laser is speed 16 mm/sec, power 80%, and corner power 10%. Make sure
the cut order for the different colors matches your intent.
Important: Make sure to select all and do "Unite Lines", and
use a tolerance of 0.01. If you don't use Unite Lines your gears will
not cut all the way through.
What to Hand In
Write your name on your prettiest spirograph drawing, take a picture
of it, and post it on Piazza under the "Spirograph Hand-in"
Collect your SolidWorks files, your DXF file, and the spirograph
drawing image you posted to Piazza into a single zip file and submit
it via Autolab by the due date shown in the syllabus.
3 points for correct SLDPRT and SLDDRW files and properly colored DXF files.
2 points for cutting the plastic and posting a spirograph drawing to Piazza.
The spur gears roll very easily around the ring gear when you put
the pen in a hole near the center. They don't roll so well when you
put the pen in a hole near the edge. Why is that?
What would you get if you put the pen in a hole that was in the
exact center of the spur gear?
Does the shape of a spirograph drawing depend on the number of
teeth in the two gears, or on the ratio of teeth in the spur
gear vs. the ring gear?
Suppose we halved the width of a tooth and doubled the number of
teeth per gear, so that the gear diameter stayed the same. What
effect would this have on the drawings we could make?
More About Gear Design
The theory of gear design is part of mechanical engineering. There
are equations for predicting the forces on gears, and for designing
optimal gear shapes. You can find some introductory material here.
The simple gears we're making are called spur gears; there are many
other kinds, such as bevel gears and helical gears. The ideal shape
for spur gear teeth uses an involute curve rather than the simple line
segments we drew by hand. Check out this flash application that
generates proper involute spur gears according to user-selectable
parameters, and even animates them:
Gear template generator and animation
You can use the equation feature of SolidWorks to automatically create
involute gear designs based on parameters such as the desired diameter
and number of teeth. It's beyond the scope of this class, but here is
a video demonstrating this technique:
Step-by-step instructions for equation-based gear design in SolidWorks
are also available at grabcad.com.
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Last modified: Fri Sep 9 18:59:54 EDT 2016