While there are a lot of shared 3D CAD models on the internet, sometime you really need to know that the model is accurate. The only sure way to do this it to create it yourself. This post will help you create accurate involute gears in SolidWorks.

To accurately generate involute curves in SolidWorks we will be using *Equation Driven Curves* in our sketches. That means we will be needing some equations, and there are quite a few for involute gears:

"DiametralPitch"= 32 "NumTeeth"= 16 "PressureAngle"= 14.5deg "Addendum"= 1 / "DiametralPitch" "Dedendum"= 1.25 / "DiametralPitch" "WorkingDepth"= 2 / "DiametralPitch" "WholeDepth"= 2.25 / "DiametralPitch" "Clearance"= 0.25 / "DiametralPitch" "ToothThickness"= 1.5708 / "DiametralPitch" "CircularPitch"= pi / "DiametralPitch" "PitchCircle"= "NumTeeth" / "DiametralPitch" "OutsideDiameter"= ( "NumTeeth" + 2 ) / "DiametralPitch" "Fillet"= "Clearance" * cos ( "PressureAngle" ) * tan ( ( 90 + "PressureAngle" ) / 2 ) "AddendumCircle"= "PitchCircle" + ( 2 * "Addendum" ) "DedendumCircle"= "PitchCircle" - ( 2 * "Dedendum" ) "BaseCircle"= "PitchCircle" * cos ( "PressureAngle" ) "PitchAngle"= 360deg / "NumTeeth" "Alpha"= sqr ( "PitchCircle" ^ 2 - "BaseCircle" ^ 2 ) / "BaseCircle" * 180 / PI - "PressureAngle" "Beta"= ( "PitchAngle" / 4 - "Alpha" ) "Phi"= sqr ( ( "AddendumCircle" / 2 ) ^ 2 - ( "BaseCircle" / 2 ) ^ 2 ) / ( "BaseCircle" / 2 )

The first three equations: *DiametralPitch*, *NumTeeth*, and *PressureAngle* will vary depending on the particular part and you will need to determine their values before we begin. With the math out of the way, let’s get started.

- Select
*Tools*/*Equations…* - In the Equation dialog change
*Angular equation units*to*Degrees* - Enter each of the above equations into the table into the
*Global*category

**-or-**

download the equations and select*Import*to add them to the table

(click the rebuild icon to resolve any errors) - Select
*OK*to exit the dialog - Select
*Insert*/*Boss/Base*/*Extrude…*to create a cylindrical gear blank- select a plane or face to start the gear
- sketch a circle and dimension the diameter to
*=”OutsideDiameter”* - exit the sketch
- extrude boss to the face width of your gear
- select
*OK*

- Select
*Insert*/*Cut*/*Extrude…*to begin the tooth gullet- select the end face of the cylinder for the starting surface
- Sketch four construction circles concentric with the OD of the boss
- dimension the circles to:

*=”OutsideDiameter”*

*=”PitchCircle”*

*=”BaseCircle”*

*=”DedendumCircle”*

- Create the upper involute curve
- select
*Tools*/*Sketch Entities*/*Equation Driven Curve* - choose Parametric
- for Equation
*x*enter_{t}

`"BaseCircle"/2*(cos(t+"Beta"*pi/180)+t*sin(t+"Beta"*pi/180))`

- for
*y*enter_{t}

`"BaseCircle"/2*(sin(t+"Beta"*pi/180)-t*cos(t+"Beta"*pi/180))`

- set Parameter
*t*to_{1}`0`

- set Parameter
*t*to_{2}`"Phi"`

- select OK to create the curve
- add a
*Fix*relation to the newly created parametric curve

- select
- Create the lower involute curve
- select
*Tools*/*Sketch Entities*/*Equation Driven Curve* - choose Parametric
- for Equation
*x*enter_{t}

`"BaseCircle"/2*(cos(-t-"Beta"*pi/180)-t*sin(-t-"Beta"*pi/180))`

- for
*y*enter_{t}

`"BaseCircle"/2*(sin(-t-"Beta"*pi/180)+t*cos(-t-"Beta"*pi/180))`

- set Parameter
*t*to_{1}`0`

- set Parameter
*t*to_{2}`"Phi"`

- select OK to create the curve
- add a
*Fix*relation to the newly created parametric curve

- select
- Create the lower portion of the tooth gullet
- add a radial construction line from the dedendum center towards the beginning of the upper involute curve ending at the dedendum circle
- add a line from the end of the previous construction line to the beginning of the upper involute curve
- add a
*Collinear*relation to both lines

- Repeat step 9 for the lower involute curve
- Cap the top and bottom of the gullet with arc segments
*Tangent*(SolidWorks seems to have a problem with the*Coradial*relation in this case) with the dedendum circle (base circle if smaller) and outside diameter - Exit the sketch
- Select
*Through All*for the extrude cut End Condition and select*OK*to cut the tooth gullet - Select
*Insert*/*Features*/*Fillet/Round…*- select
*Manual* - set
*Constant Size Fillet*type - for Parameters select
*Symmetric*and for*Size*enter*=”Fillet”* - select the two edges along the dedendum circle for
*Items To Fillet* - select OK to create the root fillets

- select
- Select the Cut-Extrude and the Fillet features from the feature tree
- then select
*Insert*/*Pattern/Mirror*/*Circular Pattern…* - set the
*Pattern Axis*to the cylinder OD face *Angle*should be 360°- for
*Number of Instances*enter*=”NumTeeth”* - select
*OK*to create the gear teeth

- then select
- Add a bore, keyway, setscrews, and hubs or other items to complete your gear

**Note: On gears with a large number of teeth, the dedendum circle will sometimes become larger than the base circle. If this is the case on your gear, skip steps 9 and 10.**