In the design of mining machinery products, a series of gears are frequently used to transmit power. When creating a three-dimensional gear model using Pro/E software, it is not only possible to realistically reflect the tooth surface geometry, but also to obtain gears with different modules, different numbers of teeth, different modification coefficients, and different pressure angles by modifying necessary technical parameters through the software’s dimension-driven capability. This approach forms a gear series. The three-dimensional design of involute gear tooth surfaces is very complex, and the work becomes extremely heavy when dealing with a series of gear solid models with different tooth numbers, modules, and modification coefficients. Because Pro/E adopts a parametric design mode, once the parameters for the number of teeth, module, modification coefficient, etc., are created, modifying different parameters can directly generate a series of gear models with correspondingly different parameters. This greatly reduces the design workload, shortens the design cycle, and simplifies the design process. In this paper, I will briefly describe the parametric design process of a straight spur gear using Pro/E, based on my own practice and experience.
General Method of Parametric 3D Design for Straight Spur Gear
There are two key issues in generating a 3D solid model of a straight spur gear: (1) how to generate the involute curve of the tooth surface, and (2) how to achieve parametric design of the gear. The specific operation steps of parametric gear design are systematically summarized in the following table.
| Step | Description |
|---|---|
| 1 | Establish gear model parameters (number of teeth, module, pressure angle, etc.) |
| 2 | Establish relational equations between parameters and sketch dimensions |
| 3 | Generate the involute curve using the equation method |
| 4 | Create the cylindrical solid of the addendum circle |
| 5 | Cut a single tooth slot using the involute profiles |
| 6 | Pattern the tooth slot around the axis and add relational equations |
| 7 | Modify the program content of the model to allow parameter input |
| 8 | Regenerate the model by changing parameters to obtain a new gear |
Establishing Gear Model Parameters
The gear model parameters that I define include: number of teeth \(z\), module \(m\), standard pressure angle \(\alpha\), addendum coefficient \(h_a^*\), radial clearance coefficient \(c^*\), and facewidth \(B\). I open the parameter dialog box by selecting Tools → Parameters in the Pro/E menu, and add the five system parameters as shown in the table below.
| Parameter Name | Value | Description |
|---|---|---|
| alpha | 20 | Standard pressure angle (degrees) |
| m | 2 | Standard module (mm) |
| z | 30 | Number of teeth |
| ha | 1 | Addendum coefficient |
| c | 0.25 | Radial clearance coefficient |
| B | 15 | Facewidth (mm) |
Creating Four Sketch Circles
I draw four concentric circles on the FRONT datum plane representing the addendum circle, pitch circle, dedendum circle, and base circle. Each circle’s diameter is then linked to the parameters through relational equations. The diameter names are changed to da, d, df, and db respectively. The relationships I enter are shown in the table below.
| Diameter Variable | Equation | Description |
|---|---|---|
| d | $$d = m \cdot z$$ | Pitch circle diameter |
| da | $$da = d + 2 \cdot h_a \cdot m$$ | Addendum circle diameter |
| df | $$df = d – 2 \cdot (h_a + c) \cdot m$$ | Dedendum circle diameter |
| db | $$db = d \cdot \cos(\alpha)$$ | Base circle diameter |
After entering these relations, the sketch circles are automatically updated to the correct sizes.
Generating the Involute Curve Using Equation
To create the involute profile of the straight spur gear, I use the Insert → Model Datum → Curve option and select “From Equation”. I choose the default coordinate system and cylindrical coordinates. The parameter equation I input into the Notepad is as follows:
| Variable | Expression | Description |
|---|---|---|
| r | $$r = \frac{db}{2 \cos(55t)}$$ | Radial distance from origin to a point on the involute |
| theta | $$\theta = \tan(55t) \cdot \frac{180}{\pi} – 55t$$ | Angle in degrees (the involute angle parameter) |
| z | 0 | Height coordinate (zero for planar curve) |
Here, \(t\) is a system variable that varies from 0 to 1. The base circle radius \(r_b = db/2\). The value \(55\) is chosen to cover the entire involute region beyond the base circle. After generating the curve, I obtain the involute shape as shown conceptually in the figure below.
Creating the Mirror Image of the Involute
In order to form one side of a tooth slot, I need to mirror the involute curve. The steps are as follows:
- Create a datum point (PNT0) at the intersection of the pitch circle and the involute curve.
- Create a datum axis (A_1) through the intersection of the TOP and RIGHT datum planes, which will be the gear center axis.
- Create a datum plane (DTM1) through axis A_1 and point PNT0.
- Create a second datum plane (DTM2) by rotating DTM1 about axis A_1 by an angle given by the formula: $$\text{angle} = \frac{360}{4z}$$. This plane serves as the mirror plane.
- Mirror the involute curve about DTM2 to obtain the opposite side of the tooth slot.
The angle formula ensures that the mirrored involute is positioned symmetrically with respect to the tooth centerline. For a straight spur gear with 30 teeth, the angle is \(360/(4 \times 30) = 3^\circ\).
Creating the Cylindrical Solid (Addendum Cylinder)
I use the extrude (add material) feature. On the FRONT plane, I sketch a circle that is coincident with the addendum circle curve (da). The extrude depth is set equal to the facewidth B. After completion, I have a solid cylinder representing the gear blank.
Creating a Single Tooth Slot (Cut Material)
Using the extrude (cut material) feature, I sketch a closed profile on the FRONT plane that exactly matches the tooth space. The profile is bounded by the two involute curves (original and mirrored), the addendum circle arc, and the dedendum circle arc. A small fillet of radius 0.2 mm is added at the root. The cut depth is set to go through the entire cylinder (same as B). This operation removes material to form one tooth slot.
Pattern the Tooth Slot
I select the cut feature and use the Edit → Pattern command. In the pattern control panel, I choose “Axis” pattern type, select datum axis A_1 as the reference, set the total angle to 360°, and the number of pattern instances initially to 30. Later I will link the pattern count to the parameter \(z\) using a relation.
Adding Relational Equations for Pattern and Reference Planes
After creating the pattern, I open the Tools → Relations dialog. In the model tree, I select DTM2, the pattern feature, and the cylindrical solid feature. The dimensions that appear are assigned to system variable names. I add the following relations to make the model fully parametric.
| Dimension Variable | Relation | Description |
|---|---|---|
| p18 | $$p18 = z$$ | Pattern instance count equals number of teeth |
| d5 | $$d5 = \frac{360}{4z}$$ | Mirror plane offset angle |
| D6 | $$D6 = B$$ | Extrude depth equals facewidth |
With these relations, any change to \(z\) or \(B\) will automatically update the pattern count, the mirror angle, and the cylinder depth.
Modifying the Program Content to Allow Parameter Input
To enable easy modification of the gear parameters without entering the relation editor every time, I modify the model program. I go to Tools → Program → Edit Design. In the Notepad window that opens, I find the section between INPUT and END INPUT and add the following lines:
m NUMBER
z NUMBER
B NUMBER
alpha NUMBER
ha NUMBER
c NUMBERAfter saving and closing the Notepad, the program is updated. Now, each time I regenerate the model, the system prompts me to input values for these parameters.
Generating a New Straight Spur Gear by Modifying Parameters
To demonstrate the parametric capability, I click the Regenerate command. The program menu appears, and I choose “Input” to select the parameters I wish to change. For example, I set module \(m = 4\) and number of teeth \(z = 60\), while keeping other parameters unchanged. After entering the values, the model regenerates and I obtain a new straight spur gear with the updated dimensions. The entire process—from adjusting parameter values to obtaining a new solid model—takes only a few seconds, significantly reducing design time for gear series.
Conclusion
By utilizing the dimension-driven and parametric design capabilities of Pro/E, and relying on a rational setup of system parameters and accurate relational equations, I can easily generate a family of similar parts—straight spur gears with varying modules, tooth numbers, and facewidths—by simply modifying a few input parameters. This parametric three-dimensional design approach tremendously reduces the repetitive and tedious work involved in the actual design of mining machinery components. It makes the design process more intuitive, concise, and convenient. The method described here is equally applicable to other types of gears, such as helical gears and bevel gears, with appropriate modifications to the underlying equations. Through this work, I have demonstrated that parametric modeling is a powerful tool for modern mechanical design, especially when a series of standard components is required.