Friday, March 6, 2020

Easier Way to Make Involute Bevel Gears in Autodesk Inventor

I have a long-winded way to make working bevel gears with involute tooth shapes for 3D printing here, but it's so long and such a pain in the butt that I thought an easier way is in order, so I streamlined the process.  I'm using Inventor 2019, by the way.  Here we go:

1) Make a new assembly and save it.
2) In that new assembly click the Design tab, then click Spur Gear.
3) Click the More Options >> button in the bottom right corner to expand the Spur Gears Component Generator window down.
4) Change Size Type to Module (if you're in my CAD 2 class, otherwise feel free to use Diametral Pitch).  Change the Input Type to Number of Teeth.
5) Change Design Guide to Center Distance.  Make sure the Internal checkbox is not checked.  Use a pressure angle of 20°, and a Helix angle of 0°.  Change your Module to 1mm, which is the smallest teeth I get a good result with on my 3D printer.
6) Type in the number of teeth you want on your smaller gear in the Gear1 area, then type in the number of teeth you want on your larger gear in the Gear2 area.
7) Hit Calculate.  If you hit the little >> bar on the right side of the window it will show you data about the gears it's going to make.
8) Click OK.  It will give you an error.  I've never had it not give me an error that says my gears won't work, but they always seem to anyway.
9) Inventor will put your gears in the assembly.  The teeth are not involute and overlap the teeth on the mating gear, so you can't use these parts in real life.
10) Right click on either of these gears and then choose Export Tooth Shape.
11) Choose the Pinion to export (which is Gear1).
12) If your 3D printer makes parts slightly too large (mine does) you will want to change your  Normal Backlash to .006, which is the largest Inventor will allow you to enter with a module of 1mm.
13) Hit ok.
14) Inventor will make an extrusion of a circle with a sketch on the end of it showing the space between the teeth.  Delete that extrusion, but leave the sketch.
15) Edit that sketch and delete the construction line circles (but not the solid outside circle).
16) In that sketch make a circular pattern of the space-between-the-teeth-shape, for however many teeth you have.
17) Trim the outside circle between each tooth so that it looks like a gear.
18)  Finish that sketch.
19) Click the Manage tab.
20) Click Parameters.
21) Click Add Numeric.
22) Type OtherGearTeeth as the new parameter name.  No spaces.  Capitalization is important.
23) Click the Unit/Type cell in that row, click the + next to Unitless, then choose Unitless (ul) and click OK.
24) In the Equation cell for that row, type in the number of teeth in the OTHER gear.  You will notice that there is already a parameter called NumberOfTeeth with the number of teeth in THIS gear, so make sure you enter the number of teeth in the gear that this gear is going to mate with.
25) Click Done.
26) Make a new sketch on the YZ Plane (which can be found under the Origin folder in the Model bar on the left side of the screen).
27) You should see the side of your gear sketch going through the origin, so it will look like a dotty line running up and down.
28) Now you are going to draw the following lines:
Make sure you don't accidentally make the two green lines perpendicular to each other.

29) Use the following picture to place the next 4 dimensions.  You can cut and paste these formulas into your dimension editing boxes.
29a) The angle between the left angled line and the centerline is:
90-(( 90 deg - atan(OtherGearTeeth / NumberOfTeeth) ) / 2 ul)

29b) The angle between the construction line and the centerline is:
90 deg - atan(OtherGearTeeth / NumberOfTeeth)

29c) The diameter between the centerline and the very bottom point of the two solid lines is:
HeadDiameter + .001

29d) The diameter between the centerline and the bottom of the construction line is:

30) Everything should be fully constrained now, so finish your sketch.
31) Revolve that triangle around the centerline.
32) Click Start 3D Sketch.
33) Click Project to Surface.
34) The "gear sketch end" of your cone is the Faces, and the sketch of the gear is the Curves.  You can just click on the end of the cone, but you have to use a bounding box to select the gear sketch. It seems to work best if you don't include the entirety of the near end of the cone in the bounding box along with the gear sketch.  Click OK.
35) Click Finish Sketch.
36) Click Axis and make an axis right through the middle of the cone.
37) Under Point, choose Intersection of a Plane/Surface and a Line, and make the surface the "non-gear-sketch-end" of the cone, and the line will be the axis you just made through the middle of the cone.
38) Click Loft, and as your first sketch choose the projected 3D sketch of the gear, and as your second sketch choose the point we just made at the other end of the cone.
39) Sometimes Cut works for the loft, and sometimes Intersect works, and I can't tell why it's not consistent, but one or the other will work.  You may have to try it both ways.  I try Intersect first usually.
40) Now you have a bevel gear.  You will need to trim it up to get it to fit into your model, but it should have the correct teeth.   Don't forget to save your work!
41) The process is exactly the same for the mating gear, but remember when you're adding the OtherGearTeeth parameter for the second gear, you won't type the same number of teeth into it as you did this time (unless both gears have the same number of teeth)


  1. The "Export Tooth Shape" option is not available in Inventor 2020 as far as I can tell.

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