My research focuses on the design and development of a computer-aided design system for the tooth modification of straight bevel gear. The work is supported by the provincial natural science foundation and the science and technology development plan. The primary objective is to integrate the tooth modification theory of straight bevel gear with a parametric modeling and assembly environment, thereby enabling rapid and accurate modification research. In this thesis, I present a systematic approach to developing a dedicated design system using SolidWorks 2010 as the supporting platform, C# as the programming language, and Visual Studio 2008 as the integrated development environment. The system comprises three main functional modules: parametric modeling of straight bevel gear, automatic assembly of straight bevel gear pairs, and tooth modification of straight bevel gear. Additional auxiliary functions include data storage and CAM/CAE interfaces. Through the application of the system to a gear pair used in automotive differentials, I validate the accuracy, reliability, and efficiency of the proposed design system.
Introduction and Motivation
Straight bevel gear is widely used in intersecting shaft transmission, particularly in automotive differentials, mining machinery, and various industrial applications. The standard involute straight bevel gear often suffers from vibration, noise, and non-uniform load distribution during meshing, caused by manufacturing errors, assembly errors, and elastic deformation under load. Tooth modification is an effective approach to alleviate these problems without substantially increasing manufacturing costs. While extensive research has been conducted on the modification of spur gears and helical gears, the modification theory for straight bevel gear is still not fully mature. Moreover, the complex three-dimensional topology of straight bevel gear makes manual modeling extremely tedious and error-prone. Consequently, there is a strong need for a dedicated design system that can support the parametric modeling, assembly, and modification of straight bevel gear, thereby facilitating the study and application of modification theory.
My research group has previously proposed the concept of tooth-direction equal-distance modification for straight bevel gear. This method generates a new tooth surface that is equidistant from the original spherical involute surface. Through dynamic finite element analysis using ANSYS/LS-DYNA, the effectiveness of this modification was preliminarily verified. Further work using orthogonal experimental optimization identified the optimal modification parameters. However, the manual creation of three-dimensional models and the subsequent modification steps for each parameter combination is highly repetitive and time-consuming. Thus, the development of a design system that automates these processes becomes essential. In this thesis, I report the design, implementation, and validation of such a system.
Development Platform and Methodology
Secondary Development of SolidWorks
SolidWorks provides a rich application programming interface (API) that allows developers to extend its functionality. The secondary development approach adopted in this work is an external mechanism, where a standalone program communicates with SolidWorks through COM/OLE interfaces. The C# language, running on the .NET Framework, offers a modern object-oriented programming model with strong integration capabilities. Visual Studio 2008 provides an efficient integrated development environment with features such as IntelliSense, debugging tools, and a visual form designer. The combination of these tools enables the creation of a plug-in that integrates seamlessly into the SolidWorks menu system.
The development platform requires installation of SolidWorks 2010, Visual Studio 2008, and the SolidWorks API SDK. I used the “SwCsharpAddin” template to create a new project, resulting in a dynamic link library (DLL) that appears as a plug-in in the SolidWorks add-in manager. After loading the plug-in, a new menu titled “Straight Bevel Gear Design System” appears in the SolidWorks menu bar. The menu contains three submenus: modeling module, assembly module, and modification module, as shown in the figure below.
Macro Recording and API Functions
To reduce development effort, I employed the macro recording capability of SolidWorks. All modeling, assembly, and modification operations are recorded as macro code. The recorded code is then transferred into the Visual Studio project and modified to use variables and parameters provided by the user interface. The key API functions are invoked in the C# code, allowing the program to drive SolidWorks operations programmatically. For operations that cannot be fully automated due to the complex geometry of straight bevel gear, I introduced human-computer interaction. For example, the system prompts the user to pick specific points, lines, or faces on the model using the mouse. The selected coordinates are then transmitted back to the program, enabling the completion of operations such as surface trimming and surface extension. The following code snippet illustrates the use of the selection manager:
$$ \text{PointArray} = \text{SelectionMgr.GetSelectionPoint2}(1, -1); $$
The returned array contains the x, y, and z coordinates of the picked point. These coordinates are converted into double values and used in subsequent modeling operations.
Overall System Design
Requirement Analysis and Functional Design
The design system must fulfill the following primary requirements:
- Rapid and accurate parametric modeling of straight bevel gear based on user-provided basic parameters.
- Automatic assembly of a straight bevel gear pair, including planetary gear and side gear.
- Assistance in tooth modification of straight bevel gear, including both tooth-profile modification and tooth-direction modification.
- Data storage for gear parameters and interfaces to CAM/CAE software for downstream analysis.
Based on these requirements, the system is divided into three basic functional modules: the modeling module, the assembly module, and the modification module. The modeling module is the foundation. The assembly module uses the generated gear models to create an assembled gear pair. The modification module applies the desired tooth modification to the selected gear. Additionally, auxiliary modules provide data storage and CAM/CAE connectivity.
Logical Architecture
The logical architecture is shown in the following table:
| Layer | Components | Function |
|---|---|---|
| User layer | Menus, dialog boxes, message boxes | Interaction between user and system |
| Application service layer | Parameter calculation, modeling logic, assembly logic, modification logic | Processing user input and executing operations |
| Support layer | SolidWorks API, DLL loading, graphics display | Low-level support for modeling and user interface |
The overall workflow is as follows: the user inputs basic gear parameters through the input interface; the system calculates indirect parameters and displays them. After the user confirms or modifies these parameters and inputs shape parameters, the system generates the straight bevel gear model through a parametric modeling process aided by human-computer interaction. The user can then invoke the assembly module to assemble the planetary gear and the side gear. The assembled gear pair can be exported to ANSYS for finite element analysis to determine the optimal modification amount. Using this amount, the user selects the modification type and parameters in the modification module. The system then performs the modification automatically or semi-automatically. Finally, the modified gear pair is reassembled and analyzed to verify the modification effect.
Detailed Design of the Modeling Module
User Interface
The modeling module provides several user interfaces: the basic parameter input dialog, the indirect parameter and shape parameter dialog, and the human-computer interaction interface. The basic parameter dialog allows the user to input the number of teeth, module, pressure angle, shaft angle, and the type of tooth depth (equal clearance or non-equal clearance). The indirect parameter dialog displays calculated values such as pitch diameter, cone distance, addendum circle diameter, dedendum circle diameter, pitch cone angle, face cone angle, and root cone angle. Some of these parameters can be edited by the user. The shape parameters include the bore diameter, the sphere radius of the planetary gear, and the boss height of the side gear.
For the gear pair considered in this thesis, the basic parameters are listed in Table 1 and Table 2 below.
| Parameter | Symbol | Unit | Value (Pinion) | Value (Gear) |
|---|---|---|---|---|
| Number of teeth | Z | – | 10 | 15 |
| Large-end module | m | mm | 4.438 | |
| Face width | b | mm | 12 | |
| Addendum coefficient | ha* | – | 0.9306 | |
| Clearance coefficient | c* | – | 0.22056 | |
| Pressure angle | α | ° | 22.5 | |
| Shaft angle | Σ | ° | 90 | |
| Profile shift coefficient | X | – | 0.1915 | -0.1915 |
| Tangential shift coefficient | Xt | – | 0 | |
Parameter Calculation
When the user inputs the basic parameters, the system automatically calculates the indirect geometric parameters according to the standard formulas for straight bevel gear. For the sample gear pair, the calculated values are presented in Table 2.
| Parameter | Symbol | Unit | Pinion | Gear |
|---|---|---|---|---|
| Pitch diameter | d | mm | 44.38 | 66.57 |
| Pitch cone angle | δ | ° | 33.69 | 56.31 |
| Cone distance | R | mm | 40 ± 0.025 | |
| Addendum | ha | mm | 4.98 | 3.28 |
| Dedendum | hf | mm | 4.19 | 5.889 |
| Whole tooth height | h | mm | 9.17 | |
| Tip circle diameter | da | mm | 50.12 | 75.19 |
| Crown distance | Aa | mm | 30.52 | 19.46 |
| Root angle | θf | ° | 9.69 | 12.31 |
| Face angle (non-equal clearance) | θa | ° | 7.0967 | 4.6878 |
| Face cone angle | δa | ° | 46 | 66 |
| Root cone angle | δf | ° | 24 | 44 |
| Arc tooth thickness | S | mm | 7.6753 | 6.8067 |
| Chordal tooth thickness | S̄ | mm | 7.6371 | 6.7948 |
| Chordal addendum | h̄a | mm | 5.2560 | 3.3765 |
For the shape parameters, the user must input values such as the bore diameter, planetary gear sphere radius, and side gear boss height. These parameters are used in the generation of the gear blank and the central hole.
Parametric Modeling of Straight Bevel Gear
The modeling procedure is based on the exact spherical involute. The spherical involute in a rectangular coordinate system is expressed by the following equations:
$$
\begin{aligned}
x &= l \sin \phi \cos \theta \cos \phi + l \sin \theta \sin \phi \cos \phi + l \cos \theta \sin \phi \cos \phi \\
y &= l \sin \phi \sin \theta \cos \phi – l \cos \theta \sin \phi \sin \phi + l \cos \theta \sin \phi \cos \phi \\
z &= l \cos \phi \cos \theta
\end{aligned}
$$
However, the standard parametric form of the spherical involute used in the software is often written as:
$$
\begin{cases}
x = l \left( \sin \theta \cos \phi \cos \theta \psi + \sin \psi \sin \theta \cos \phi \right) \\
y = l \left( \sin \theta \cos \phi \sin \theta \psi – \sin \psi \cos \theta \cos \phi \right) \\
z = l \cos \theta \cos \theta \psi
\end{cases}
$$
where \( l \) is the radius of the sphere, \( \theta \) is the base cone angle, and \( \psi \) is a parameter. In my implementation, I used the “equation-driven curve” function of SolidWorks to create a 3D sketch of the spherical involute. The program constructs the equations as strings and passes them to the API function CreateEquationSpline2. The key code is as follows:
$$ x(\psi) = l \left( \sin \theta \cos \psi \cos(\theta \psi) + \sin \psi \sin(\theta \psi) \right) $$
$$ y(\psi) = l \left( \sin \theta \sin \psi \cos(\theta \psi) – \cos \psi \sin(\theta \psi) \right) $$
$$ z(\psi) = l \cos \theta \cos(\theta \psi) $$
with \( \psi \) ranging from \( 0 \) to \( \pi/3 \). This approach guarantees the accuracy of the tooth profile because it directly uses the spherical involute equation rather than an approximation based on the back cone or spline interpolation.
The modeling steps are as follows:
- Generate the spherical involute curve using the equation-driven curve tool.
- Create a surface by lofting the spherical involute curve from the sphere center to the outer boundary.
- Mirror the spherical involute surface with respect to the tooth profile center plane.
- Create the ruled surface between the two mirrored involute surfaces and stitch them together.
- Generate a single tooth by revolving the tooth profile and trimming with the blank surfaces.
- Array the single tooth around the gear axis to create all teeth.
- Create the gear blank by revolving the cross-section profile around the gear axis.
- Add the central bore and fillets/chamfers.
Because the coordinates of the gear blank cross-section points are derived from the geometric parameters, the program can compute these coordinates dynamically from the user inputs. For example, the points A, B, C, D, E, F, G, H, I, J, and K in the cross-section are expressed as functions of the cone angles and the dimensions. For an equal-clearance or non-equal-clearance tooth, the face angle differs, and the program uses a conditional statement to assign the correct coordinates.
Human-Computer Interaction in Modeling
During the modeling process, some surfaces and edges are not visible in the feature tree and cannot be selected programmatically. To solve this issue, the system prompts the user to pick a point on the desired face or edge. For example, after generating the spherical involute surface, the user is asked to click on the surface to allow the system to perform a surface trim. The message boxes guide the user step by step. After the user picks the required face, the system obtains the selection point and uses it to identify the correct feature. This semi-automatic approach significantly increases the robustness of the modeling module.
Detailed Design of the Assembly Module
The assembly module automatically assembles a planetary gear and a side gear of a straight bevel gear pair. The user interface, shown in the previous section, allows the user to select the gear files by browsing or by typing the file paths. After both files are selected, the system opens the gear models, creates a new assembly file, and inserts the two gears as components. The assembly constraints are defined as follows:
| Constraint Type | Entities | Relation |
|---|---|---|
| Coincident | Gear axis of planetary gear with line 1 in the assembly sketch | Coincident |
| Coincident | Gear axis of side gear with line 2 in the assembly sketch | Coincident |
| Coincident | Cone apex of planetary gear with the assembly origin | Coincident |
| Coincident | Cone apex of side gear with the assembly origin | Coincident |
| Coincident | Tooth profile center plane of planetary gear with an assembly reference plane | Coincident |
| Coincident | Tooth space center plane of side gear with the same assembly reference plane | Coincident |
| Gear mate | Planetary gear and side gear | Gear ratio = Z2/Z1 |
The assembly process utilizes the AddMate3 API function. Before adding the gear mate, the coincident constraints between the tooth profile center plane and tooth space center plane are temporarily suppressed to avoid conflict. Then a gear mate is added, allowing the gear pair to rotate relative to each other. The assembly module also includes a CAE interface button that launches ANSYS. The user can export the assembled gear pair to ANSYS for finite element analysis.
Detailed Design of the Modification Module
Types of Tooth Modification
The modification module supports two categories: tooth-direction modification and tooth-profile modification. For tooth-direction modification, the system implements the equal-distance modification method. For tooth-profile modification, the system implements linear profile modification. The module provides a user interface for selecting the gear file and the modification type, as well as parameter input dialogs.
Tooth-Direction Equal-Distance Modification
The equal-distance modification is applied to the tooth surface of a straight bevel gear by creating a new surface that is offset by a constant amount along the normal direction to the original spherical involute surface. This new surface remains a spherical involute surface and replaces the original tooth surface in the contact region. The geometric construction involves the creation of a quadrilateral on the tooth profile center plane. The four sides of this quadrilateral are parallel to the four sides of the tooth cross-section ABCD, as shown in the schematic. The position and size of the quadrilateral are determined by the modification region parameters, i.e., the distances from the tooth edges. The modification amount is the offset distance.
To parameterize the modification region, I derived the coordinates of the four corners of the quadrilateral as functions of the gear basic parameters and the modification parameters. For instance, the coordinate of point a is obtained by solving the equations of two adjacent lines after offsetting the original lines AB and AD by the given distances. The general formula for the line offset is:
$$
\text{Line equation after offset: } A x + B y + C + k \sqrt{A^2 + B^2} = 0
$$
where \( A \), \( B \), \( C \) are the coefficients of the original line, and \( k \) is the signed distance. After obtaining the coordinates of the quadrilateral corners, the program creates a sketch on the tooth profile center plane and performs an extruded boss feature. The extrusion termination condition is set to “up to surface” with the offset distance equal to the modification amount. To reduce stress concentration at the corners, fillets are added to the quadrilateral vertices. Then, the extruded feature is mirrored and arrayed to every tooth surface. The user can choose to enter the modification parameters manually or select the default parameters. For the sample gear, the optimal modification amount obtained from prior finite element analysis is 25 micrometers.
The modification module user interface is shown in the following figure description. When the user selects “tooth-direction equal-distance modification,” the system prompts the user to pick a point on the tooth face to identify the specific tooth surface. After the point is selected, the system automatically performs the extrusion, mirror, and array operations.
Tooth-Profile Linear Modification
Tooth-profile linear modification is performed by removing a thin layer of material from the tooth profile in the tip region or the root region. The modification is defined by a start line and an end line on the tooth surface, and the modification amount is linearly varying along the profile. The process is semi-automatic due to the complexity of the spatial geometry. The system guides the user through the following steps:
- The user defines the line AB at the small end of the tooth profile.
- The user defines the line CD at the large end of the tooth profile.
- The system creates a lofted surface between AB and CD.
- The system extends the lofted surface and uses it to cut the tooth surface.
- The system mirrors and arrays the cut feature to complete the modification.
To assist the user, the system automatically rotates the model to a convenient viewing angle and displays a message box with instructions. The user clicks on the model to draw the lines using SolidWorks’ sketch tools. After each step, the user clicks the corresponding button in the human-computer interaction interface. The modification parameters, such as the modification length and modification amount at the small and large ends, are entered in the parameter dialog box. The system validates the parameters to ensure they are within reasonable ranges.
Data Storage and CAM/CAE Interfaces
The design system includes a data storage component that saves all gear parameters into a database. The user can click the “store data” button in the parameter dialog to store the basic, indirect, and shape parameters. The stored data can be viewed in a separate interface with multiple tabs, such as “basic parameters,” “planetary gear parameters,” and “side gear parameters.” The database is implemented using Microsoft Access or an embedded database through C#. This feature is useful for documentation and for later reference.
The CAM/CAE interfaces provide the following capabilities:
- The modeling module has a “Cimatron” button that launches Cimatron CAM software. This enables the user to directly import the generated straight bevel gear model for computer-aided manufacturing.
- The assembly module has an “ANSYS” button that launches ANSYS finite element analysis software. This allows the user to import the assembled gear pair for stress analysis, dynamic analysis, and verification of the modification effect.
These interfaces significantly enhance the practicality of the design system by connecting the CAD model with downstream analysis and manufacturing tools.
System Application and Validation
Parametric Modeling Example
I applied the design system to model the straight bevel gear pair used in a car differential. The basic parameters were entered in the basic parameter dialog as shown in the previous section. After clicking the “calculate” button, the indirect parameters appeared in the dialog. I then modified the relevant parameters and input the shape parameters for the planetary gear and the side gear. The system generated the gear models through a series of human-computer interactions. The resulting planetary gear and side gear models were compared with the manually created models from my research group. The comparison showed that all the relevant dimensions were exactly identical, confirming the accuracy of the parametric modeling. The modeling time was reduced from more than an hour for manual modeling to just a few minutes with the design system.
Automatic Assembly Example
After modeling the two gears, I launched the assembly module. I selected the planetary gear file and the side gear file by browsing. The system then opened both files, created a new assembly, inserted the components, and automatically added the mating relationships. The complete assembly of the straight bevel gear pair was generated in a few seconds. Figure 5.12 in the thesis shows the assembled gear pair. The gear pair meshing was checked by adding a gear mate and rotating one gear; the meshing was smooth and correctly oriented in the perpendicular shaft arrangement.
Tooth-Direction Equal-Distance Modification Example
To verify the modification module, I selected the planetary gear and the equal-distance modification option. The modification amount was set to 25 micrometers based on previous optimization. The modification region parameters were set to the default values obtained from the design table. After clicking the command to start modification, the system automatically adjusted the view and prompted me to pick a point on the tooth face. After clicking, the system created the offset tooth surface on all teeth. The result is shown in Figure 5.16 of the thesis. By visually inspecting the modified tooth surface, I could observe a clear offset layer near the tooth flank. I then assembled the modified gear with the side gear and exported the assembly to ANSYS. The finite element analysis indicated that the contact stress distribution was more uniform and the maximum stress was reduced compared with the unmodified gear, confirming the effectiveness of the equal-distance modification.
Tooth-Profile Linear Modification Example
For the tooth-profile modification, I selected the planetary gear and the linear profile modification type. The modification parameters were entered according to the research group’s recommendations. The system guided me through the four-step process: defining the line AB at the small end, defining the line CD at the large end, generating the lofted surface, and completing the cut. The process required some manual sketch work, but the system provided clear instructions and automatically managed the model orientation. After completing the modification, the modified tooth showed a gradual removal of material near the tip, which is typical for profile modification. The entire process took about five minutes, which is significantly faster than manual modification.
Conclusions and Future Work
In this thesis, I have successfully developed a tooth-modification design system for straight bevel gear based on SolidWorks. The main achievements are summarized as follows:
- The design system integrates precise parametric modeling of straight bevel gear using the spherical involute equation, ensuring high tooth profile accuracy.
- The automatic assembly module significantly reduces the time required for assembling a straight bevel gear pair and provides a reliable model for further analysis.
- The modification module supports both tooth-direction equal-distance modification and tooth-profile linear modification, and it incorporates prior modification theory to provide default parameters, thus accelerating the modification process.
- The data storage and CAM/CAE interfaces make the system a complete CAD/CAM/CAE solution for straight bevel gear research and production.
Future work can focus on the following aspects:
- Enhancing the tooth-profile modification module to support graphical curve modifications such as parabolic or circular arc modification.
- Implementing automatic finite element analysis within the design system, eliminating the need for manual ANSYS operations.
- Adding more varieties of straight bevel gear modifications, including longitudinal crowning and combined modifications.
- Extending the system to support other types of bevel gears, such as spiral bevel gears and hypoid gears.
Overall, the developed system demonstrates a practical and efficient approach to the design and modification of straight bevel gear, and it provides a strong foundation for further research and industrial application.