Five gears with different sizes

Making Gears with Hobby CNC

I made aluminum spur gears of module 0.5 and up using hobby CNC. First, I used SOLIDWORKS and involute curve formula to model the part. Then, I used Fusion 360 and KitMill RZ300 to fabricate the part.

Making CSV File of Tooth Curve Position Data

Screenshots of Excel and CSV

Input: Gear Parameters

Module m 0.5
Number of Teeth N 8
Pressure Angle α 20°

Output: Involute Curve

Involute curve parametric equations


Pitch Diameter D = Nm
Base Diameter Db = Dcosα
Involute curve graph

Pitch diameter is sometimes called reference diameter. For my example, I used t = 0 to 2 with increment of 0.05. First column is X, second is Y, and third is Z.

XYZ position list in Excel

Making 3D Model in SOLIDWORKS

Gear diagram showing dedendum circle, base circle, pitch circle, addendum circle and their respective diameters, Da, D, Db, Dd, and quarter circular pitch
Tip Diameter Da = D + 2m
Root Diameter Dd = D − 2.5m
Circular Pitch p = πm

In the following steps, I am using SOLIDWORKS 2009 to import the CSV file and make gear model using it. SOLIDWORKS 2012 and newer and some other CAD softwares support creating curves directly by inputting parametric equations in which case the CSV file is not needed.

Features > Curves > Curve Through XYZ Points

SOLIDWORKS screenshot of Curve Through XYZ Points button

Browse... > Change file type from "Curves (*.sldcrv)" to "Text Files (*.txt) > Open > OK.

SOLIDWORKS screenshot of Curve File window

The CSV file extension needs to be ".txt" and not ".csv". If SOLIDWORKS displays error "The data in this file may be invalid." make sure that,

Sketch in Front Plane, select Curve.

SOLIDWORKS screenshot of Curve Through XYZ Points button

Sketch > Convert Entities.

SOLIDWORKS screenshot of Convert Entities button

Sketch four circles: dedendum circle, base circle, pitch circle, and addendum circle. Base circle touches the involute curve at t = 0.

SOLIDWORKS screenshot of root, base, pitch, and tip circles sketch

Sketch two straight lines. Dimension quarter pitch arc by clicking the pitch circle and then two points on the sides.

SOLIDWORKS screenshot of quarter pitch sketch

Exit Sketch, Features > Extruded Boss/Base, select tip circle, check.

SOLIDWORKS screenshot of extruding tip circle

Select Sketch in Extrude, Features > Extruded Cut.

SOLIDWORKS screenshot of Extruded Cut button

In "Selected Contours", select regions to be removed, check.

SOLIDWORKS screenshot of regions for Extruded Cut

Features > Circular Pattern.

SOLIDWORKS screenshot of Circular Pattern button

Number of Instances: Number of Teeth (8 in example), Features to Pattern: Extruded Cut feature, check.

SOLIDWORKS screenshot of Circular Pattern parameters

Features > Mirror.

SOLIDWORKS screenshot of Mirror button

Mirror Face/Plane: flat face in extruded section, Features to Mirror: Circular Pattern feature, check.

SOLIDWORKS screenshot of Mirror parameters

Final model:

SOLIDWORKS screenshot of final gear model

Making CNC Toolpath in Fusion 360

I calculate .

Machining with Hobby CNC

I calculate .