How to model spur gear in CAD

This topic explains how to model a spur gear in Pro engineer and Creo without gear relations except for the involute curve.

Normally the following parameters are enough to manufacture a spur gear.

1. Number of Teeth

2. Module

3. Pressure Angle

4. Width

All other necessary parameters like pitch circle dia, root dia, base circle diameter etc. are derived by standard set of gear formulas using these values.

But sometimes the manufacturer may have changed some of the values of a gear pair to satisfy his own requirement. In this case, a table containing all the parameters is placed in the gear drawing. This data is used to manufacture the gear. The job of the Cad modeler will be to create the gear model using these values.

Lets see how to model the gear using the data given in the table (see left). To model the gear completed using gear formulas read here.

You can download the gear drawings from the Downloads-Cad page.

Normally the following parameters are enough to manufacture a spur gear.

1. Number of Teeth

2. Module

3. Pressure Angle

4. Width

All other necessary parameters like pitch circle dia, root dia, base circle diameter etc. are derived by standard set of gear formulas using these values.

But sometimes the manufacturer may have changed some of the values of a gear pair to satisfy his own requirement. In this case, a table containing all the parameters is placed in the gear drawing. This data is used to manufacture the gear. The job of the Cad modeler will be to create the gear model using these values.

Lets see how to model the gear using the data given in the table (see left). To model the gear completed using gear formulas read here.

You can download the gear drawings from the Downloads-

There are two cases. The root diameter can be larger than the base diameter or the base diameter may be larger than root diameter. There are some changes in modeling the two cases. We will see that one by one.

Root diameter is larger than base diameter (see table):

1. Make a circle with 149.70 (Root diameter) and extrude it for 50 mm (Width).

1. Make a circle with 149.70 (Root diameter) and extrude it for 50 mm (Width).

2. Create three circles in the front face of the gear blank and name it in the model tree.

Pitch diameter - 156, Base diameter - 146.59, Outer diameter - 167.4

Pitch diameter -

3. Create a new coordinate system at the center of the gear blank using the datums and front face as shown in the image. Name it “GEAR_CSYS” for reference purpose. Make sure that the Z direction points outside, X horizontally and Y vertically. I recommend to crate it as shown in the image (X and Y in positive direction). This coordinate will be used to create the involute curve from equation.

Front view

4. Now the involute curve has to be created. In ProE wildfire versions, go to Insert → Model datum → Curve or use the short cut button. This will open up the curve menu manager. Click on From equation and Done. Now you have to select the newly created “GEAR_CSYS” coordinate. Then select “Cartesian”. This will open the text window.

In Creo, type Curve in the search box at the top right corner and select “Curve from equation” from the list.

Now paste this equation in the text window.

Note: 146.59 is the base diameter.

Base_Rad = 146.59/2

Angle = t*90

Cir_len = (PI * Base_Rad * t ) / 2

X_Pnt = Base_Rad * cos(Angle)

Y_Pnt = Base_Rad * sin(Angle)

X = X_Pnt + ( Cir_len * sin(Angle))

Y = Y_Pnt - ( Cir_len * cos(Angle))

Z = 0

In Creo, type Curve in the search box at the top right corner and select “Curve from equation” from the list.

Now paste this equation in the text window.

Note: 146.59 is the base diameter.

Base_Rad = 146.59/2

Angle = t*90

Cir_len = (PI * Base_Rad * t ) / 2

X_Pnt = Base_Rad * cos(Angle)

Y_Pnt = Base_Rad * sin(Angle)

X = X_Pnt + ( Cir_len * sin(Angle))

Y = Y_Pnt -

5. Create a sketch for circular tooth thickness (6.28 - see table) at pitch diameter from the intersection point of involute curve and Pitch diameter as shown in the video..

6. Come out of the sketcher. Crate a new point at the center of the circular tooth thickness curve using point option. To do that, go to Insert → Model datum → Point → point. Now click the newly created curve and enter 0.5 in the input area as shown in the image.

7. Create a new datum using the point created in step 6 and the center axis of the gear as shown in the image. This will be used to mirror the involute curve.

8. Mirror the involute curve using the datum created in step 7.

9. Create a extrude for a single teeth. Use the two involute curves and the outer diameter and base diameter for the sketch. Trim all other entities. Extrude the sketch to the next face.

9. Create the chamfer and radius.

10. Group the Extruded teeth, chamfer and the radius in the model tree.

11. Pattern this group using the center axis of the gear. 39 teeth (No. Of teeth) for 360 degrees.

12. Add center hole, key way cut and chamfer to the teeth side faces. Thats it we have a spur gear now.

To model gear with Base diameter larger than Root diameter.

Multiple methods can be used to model the gear. Just understand the concept. You can also do it on your own way combining the steps.

Save the text window and close. Click done. This will create the involute curve.