Tutorial 3: A Meshing Spur Gear Pair

Goal#

Make two spur gears that mesh correctly and rotate together in Fusion: a 20-tooth pinion and a 30-tooth gear, both module 2 with a 20 degree pressure angle, 8 mm thick, with 8 mm bores, mounted on pins in a simple base plate. By the end you will have a working 3:2 reduction that you can drive with a Motion Link and print.

Gears are the classic case where understanding the numbers matters more than the clicking. The geometry of an involute tooth is hard to draw by hand in Fusion, so you will generate the profile with the bundled Spur Gear sample, then do everything around it (bore, hub, keyway, joints, base plate) yourself.

What you'll learn#

• The five numbers that define a gear pair: module, tooth count, pressure angle, center distance, backlash.
• Running the Spur Gear sample that ships with Fusion.
• Positioning gears by center distance, not by eye.
• Phasing the teeth so they interleave rather than collide.
• Using Revolute joints plus a Motion Link to drive gear ratio.
• Checking for interference with Contact Sets and the Interference tool.
• Printing tolerances for gears.

Prerequisites#

• Tutorials 1 and 2, or equivalent skills with sketching and extrusion.
• Components and joints from the Components and Assemblies section.
• Access to the Spur Gear sample. Autodesk's API documentation describes it as a sample that adds a command to the Create panel (Solid tab); if it is not listed in your installation, see the Scripting and API section for how to locate or install samples.

The numbers#

For metric gears, size comes from the module m, the pitch diameter divided by tooth count. A larger module means bigger teeth. Both gears must share module and pressure angle to mesh.

For 3D printing add backlash (clearance between mating teeth) of about 0.1 to 0.2 mm; the script has a field for it.

Steps#

Part A: Parameters#

1. New design. File > New Design and save as Gear Pair.
2. Add parameters. Open Modify > Change Parameters and add: m = 2 mm, z1 = 20 (no unit), z2 = 30, gear_t = 8 mm, bore_d = 8 mm, cd = m * (z1 + z2) / 2. Parameter cd should read 50 mm. You will use these values both in the script dialog (typed manually) and later in the assembly.

Part B: Generate the pinion#

3. Open Scripts and Add-Ins. Press Shift+S or go to Utilities > Scripts and Add-Ins. Find SpurGear among the sample scripts and add-ins and click Run (or use the Spur Gear command in the Create panel if the sample added it).
4. Fill in the dialog. The sample's dialog fields are not listed in Autodesk's help; the names below are those of the sample's command inputs and may differ in your version:
   • Standard: Metric
   • Pressure Angle: 20 deg
   • Module: 2
   • Number of Teeth: 20
   • Backlash: 0.15 (mm)
   • Root Fillet Radius: 0.5 (mm, helps printing and reduces stress)
   • Gear Thickness: 8
   • Hole Diameter: 8 (the bore)
5. Select the plane. Pick the XY plane (or a planar face) when asked.
6. Confirm. Click OK; the script builds the gear.
7. Result. A new component named something like Spur Gear (20 teeth) appears with a sketch containing the tooth profile and an extrusion for the body. The script creates a new component; rename it Pinion.

Part C: Generate the gear#

8. Run again. Open the script a second time with Number of Teeth 30, all other fields identical. Do not alter module or pressure angle.
9. Rename. Call the new component Gear. At this point both gears are centered on the origin and overlap each other.

Part D: Position at the center distance#

10. Ground the base. Create a new component Base Plate: sketch on XY a center rectangle 120 mm x 70 mm (the gears' tip circles reach X = -47 and +57, so a smaller plate would leave them overhanging), then extrude 4 mm downward (negative Z) so the top face is at Z = 0. Fillet the four vertical edges 5 mm.
11. Add pin holes. Sketch on the plate top. Place points at X = -25 mm and X = +25 mm, Y = 0 (50 mm apart, equal to cd). Use construction geometry to keep the points symmetric about the Y axis.
12. Pins. Make two pins: new component Pin, sketch a circle of diameter 7.8 mm on the plate top at each point (the gear bores are 8 mm, so this leaves 0.2 mm diametral, 0.1 mm radial, clearance; a typical FDM starting value, reduce it for metal rods) and extrude 14 mm up as a New Body (Z 0 to 14, taller than the 8 mm gears and 4 mm hubs).
13. Move the pinion. Right-click the Pinion component > Move/Copy, or press M. Set Move Type to Translate and enter X = -25 mm. Alternatively create a Revolute joint (below) and let it place the component.
14. Move the gear. Translate Gear by X = +25 mm.

Part E: Phase the teeth#

At this stage both gears may have teeth pointing at each other. For meshing, a tooth of one gear must sit in a gap of the other at the contact point on the line of centers.

15. Inspect. View the XY plane from above (View > Look At, or click the ViewCube Top face). Zoom to the meshing point at X = 0.
16. Rotate to phase. The rule: if the pinion has an even tooth count, a tooth tip sits on the center line facing the gear when the model is generated at the X axis. The 30-tooth gear also has a tooth on the axis. The tips collide, so rotate one gear by half a pitch: 360 deg / z / 2. For the gear this is 6 deg (360 / 30 / 2). Use Move/Copy > Rotate about the gear's own Z axis (set the pivot at the gear center), angle 6 deg.
17. Check. Run Inspect > Interference selecting both gears. Interference should list none; if tooth tips overlap by a tiny amount, increase center distance by 0.1 mm and reduce nothing else, or increase backlash.

Part F: Joints#

18. Revolute for the pinion. Press J. Choose Component 1 as the pinion (snap to the center of its bore on the front face) and Component 2 as the pin (snap to the center of the circular top edge or the axis). In the Motion tab choose Revolute; axis Z. Click OK.
19. Repeat for the gear. Revolute joint between Gear and the second pin.
20. Ground the plate. Right-click Base Plate > Ground. The pins must also be grounded or rigidly joined to the plate: use a Rigid joint or a Rigid Group.
21. Motion Link. Go to Assemble > Motion Link. Select the pinion's revolute joint and the gear's revolute joint, and give each a Value: 360 deg for the pinion and 240 deg for the gear, because the pinion has 20 teeth and the gear 30: the gear turns z1/z2 of a revolution. Use the Reverse option so the rotations are opposite.
22. Drive it. Drag the pinion; the gear follows at 2/3 speed in the opposite direction. If the motion is the same direction, flip the link.

Part G: Hubs, keyway and details#

23. Hub. Add a 16 mm diameter, 4 mm tall hub on the top (Z = 8 mm) face of each gear, away from the base plate: select that face, sketch a circle bore_d + 8 mm, extrude 4 mm, Join into the gear body.
24. Set screw hole. For metal use, add a 3 mm radial hole with Hole at the hub side face. For printed gears omit.
25. Chamfer. Press the chamfer command on the tooth tips edges of both faces, 0.3 mm, to help the teeth enter each other. Chamfers on involute teeth can be many edges; select the whole outer face loop instead.

Part H: Contact Sets and animation#

26. Contact Set. Assemble > Enable Contact Sets, then Assemble > New Contact Set and select Pinion and Gear. With contact enabled, the parts cannot pass through each other during joint drag.
27. Motion Study. Use Assemble > Motion Study to play the motion link, or drag the pinion in the Design workspace; use the Animation workspace if you want a video.

Checkpoints#

• Center distance between the two bore axes: Inspect > Measure shows 50.000 mm.
• Tip circle clearance to the other root circle: 0.5 mm (dedendum 1.25 m minus addendum m = 0.25 m); measure from the tip circle of one to the root of the other.
• Interference result empty.
• Rotating the pinion by 360 deg turns the gear 240 deg.
• Pinion and gear both show as separate components with a joint icon in the browser.

Print and tolerance guidance#

Variations#

1. Different ratio. Change z2 to 40 and rerun the script; center distance becomes 60 mm.
2. Helical gears. The same script generates straight teeth only; use a Sweep with a twisted path or switch to a tool that supports helical gears (verify before relying on it).
3. Rack and pinion. Sketch a rack tooth profile with 6.283 mm pitch and trapezoid teeth 20 degree flanks, then pattern it.
4. Three gear train. Add an idler; the ratio is unchanged but direction flips.
5. Gear cover. Make a case with the enclosure techniques from Tutorial 2.

Troubleshooting#

Related#

• Joints and Motion Study pages explain every option used above.
• Contact Sets explains collision behavior.
• Next, Tutorial 4 prints a moving mechanism in one piece.