Static and Modal Models of Automotive Wheel Hubs Based on Lightweight Design and Cost-Effectiveness

Abstract

This study investigated the optimization design methods for automotive wheel hub structures based on lightweight and economic considerations through static and modal analyses. A comprehensive static analysis and modal analysis of the automotive wheel hub were conducted using finite element analysis to understand its response characteristics under load. In order to optimize the structure of the wheel hub, the lightweight design is also considered on the premise of ensuring the reliability of its stiffness and strength. By appropriately setting the initial conditions and boundary conditions, the deformation and stress distributions of the optimized wheel hub were obtained for various loading positions. The modal analysis results showed that the vibration frequencies of the optimized wheel hub avoided external excitation frequencies, meeting the design requirements. Further analysis of the lightweight effect of the wheel hub was conducted, and a lightweight material replacement scheme was proposed. Ultimately, the rationality of the optimized wheel hub’s strength and vibration performance was validated through comprehensive static and modal analyses.

1. Introduction

With the rapid development of the automotive industry, there is an increasing demand for high-performance and safety standards in vehicles. As an important part of the automobile suspension system, the automobile wheel hub bears the weight of the vehicle and is also used to transmit power. The rationality of their structure has a significant impact on the vehicle’s performance and comfort. Additionally, in the context of the global environmental demand for reducing carbon emissions, energy-saving and emission reduction have become a prominent trend [1,2]. Therefore, the structural safety and lightweight design of wheel hubs have become increasingly important in the field of automotive manufacturing [3].

Traditional wheel hub design is often based on empirical and trial-and-error methods, lacking a comprehensive and scientific approach. However, with the development of computer technology and finite element analysis (FEA) methods, utilizing numerical simulation for analyzing and optimizing wheel hub structures has become an effective approach. More and more researchers have started using the finite element method (FEM), which not only has rigorous mathematical theory but can also solve complex nonlinear strain–stress relationships. Numerical simulation can also provide a unified direction for process optimization, reducing the number of experiments and improving experimental efficiency and success rates [4,5]. For instance, Bourden [6] proposed a method that defines the standard finite element method as a stiffness matrix, which can be used to analyze the dynamic loads and displacements of the internal rolling bearings of the wheel hub, as well as the interaction between loads and displacements.

In the optimization design of wheel hub structures, selecting the appropriate optimization method and setting reasonable parameters are key factors. It is necessary to conduct in-depth research and comparison of different optimization methods and determine the most suitable method and parameters based on the specific problem. The mass, center of gravity position, and mass moment of inertia of the wheel hub are important factors that affect the driving and steering performance of the vehicle. During the test, if the deviation caused by these factors is too large, it will have a significant negative impact on the overall motion performance of the vehicle [7]. The material properties of the wheel hub have a significant influence on its strength, stiffness, durability, and other aspects. However, there are still certain limitations and shortcomings in the performance testing of wheel hub materials, such as incomplete testing methods and imprecise experimental data. The main types of materials for wheel hubs are steel, aluminum alloy, and magnesium alloy. Aluminum alloy wheel hubs, due to their advantages of being lightweight, having good heat dissipation, high safety factor, and design flexibility, currently account for approximately 54% of the global wheel hub market [8], with approximately 80% of aluminum alloy wheel hubs being produced by LPDC [9]. In addition, by processing the modal analysis results of the wheel hub, we can obtain the natural frequency, mode shape and other parameters that affect the movement of the wheel hub, which provides a certain basis for the structure optimization, material selection and manufacturing process in the design process of the wheel hub. During modal analysis, attention should be paid to modeling errors, selection of boundary conditions, modal truncation issues, and uncertainties in material properties. Employing appropriate methods and strategies can improve the accuracy and reliability of modal analysis results. Chołodowski et al. [10] analyzed the rolling energy loss of wheels through experiments and model development, indicating that the rolling resistance of a vehicle was governed by various factors, such as the normal load. Ioannides et al. [11], based on the LP theory, proposed that when the stress load borne by the structure is lower than the fatigue endurance limit, the structure will not experience fatigue failure, thus improving the fact that the LP theory does not have an infinite life limitation.

In addition, the distributed drive motor has shown great advantages in electric vehicle applications due to its high transmission efficiency, independent and controllable torque, etc., and this drive mode is gradually becoming the optimal drive scheme for electric vehicles [12]. Yang et al. [13] took the motor efficiency MAP as the research object and adopted different optimization algorithms to realize the optimal distribution of four motor driving torques. Dizqah et al. [14] established the management of transmission power loss and vehicle demand torque, carried out research on torque distribution of four-wheel distributed drive electric vehicles, and proposed a drive distribution strategy based on analytic torque threshold. However, the above research did not comprehensively consider the driver’s driving intention of acceleration and deceleration, and there were some problems, such as low calculation accuracy of demand torque and poor dynamic performance. Later, Chen et al. [15] proposed to adopt a hierarchical structure to achieve accurate driving/braking/steering control, calculate the total force and yaw moment combined with the sliding mode control scheme, and adopt the fuzzy logic method to control the anti-skid braking system. The strategy they developed improved vehicle maneuverability in all conventional operating conditions, reduced energy consumption from motor and tire sideshows, and ultimately enabled optimal torque and angle distribution for all wire electric vehicles (FWIC-EVs). Wheel hubs are complex structural systems, and their performance is influenced by multiple factors, including structural shape, material properties, and load conditions. In order to improve the design accuracy and performance of the wheel hub, it is necessary to consider the influence of many conditions and constraints. For example, the factor error in the mechanical structure when using different motors or the synchronous control strategy of the steering-by-wire system of the dual steering actuator motor have a certain impact on the hub performance. Onoda et al. [16] designed the structure of the steering-by-wire system with two controllers and two steering executive motors. The system installed a clutch between the steering column and the steering gear, which further improved the safety of the steering-by-wire system. Based on this structure, Koizumi et al. [17] proposed a control strategy based on lateral acceleration feedback control.

In this paper, finite element analysis (FEA) is used to study the static, modal and lightweight analysis of wheel hubs after applying force at different positions. The article can be divided into four bullet points according to the simulation and validation results, including static analysis, modal analysis, optimization design, and lightweight analysis of the wheel hub. The purpose of this study is to significantly reduce the weight of the wheel hub within the safe range without affecting the performance of the wheel hub, such as deformation, mode, etc. The modified and optimized model is checked to provide a basis for evaluating the performance of the wheel hub.

2. Three-Dimensional Model and Numerical Methodology

2.1. Three-Dimensional Model

This study was conducted using a specific brand of car model. The total vehicle mass of this model was 1500 kg. Assuming it was fully loaded with five adults weighing 70 kg each and carrying 100 kg of luggage, the total mass when fully loaded was estimated to be 1950 kg. By considering the equal distribution of the support force among each wheel, the estimated support force borne by each wheel was 4777.5 N. The hub type selected in this paper was a 5° deep slot rim. The three more important parameters, including the thickness of the rim, the horizontal width of the bevel of the inner rim bead seat and the rim diameter, are 4 mm, 60 mm and 436.6 mm, respectively. The preliminary design of the spoke structure was a five-spoke plate; the section shape of the spoke was designed as a wave, and its section thickness was 35 mm, 32 mm and 30 mm in turn. The vent of the spoke adopted a fan-shaped structure with a rounded radius of 10 mm and a fan-shaped angle of 60 degrees. The position of the valve nozzle hole was on the side wall of the rim groove, and the style of the valve nozzle hole was selected. The diameter of the valve orifice was 11.3 mm, the length of the smooth cylinder was 3 mm, and the edge of the valve orifice was chamfered at 45 degrees. Figure 1 shows the three-dimensional model of the wheel hub, featuring a five-spoke design. The chosen material for the wheel hub was an aluminum alloy, specifically the ZAlSi7MgA cast aluminum alloy (designated as ZL101A). The aluminum alloy material has a density of 2.68 g/cm³, elastic modulus of 70 GPa, Poisson’s ratio of 0.33, and yield strength of 205 MPa.

2.2. Meshing Methods

Based on the analysis requirements and the geometric characteristics of the wheel hub, an appropriate grid type was selected. In this study, a non-structured grid, mainly consisting of tetrahedral elements, was used for meshing the wheel hub. The grid density was determined based on the desired analysis accuracy and computational resource limitations. In critical regions, such as areas experiencing significant loads and connections, a finer mesh was employed to obtain more accurate results and capture local behavior. Less critical regions can be meshed with relatively coarser elements. The ANSYS ICEM 19.2 was used for meshing the geometric model of the wheel hub. Three different grid densities were employed, resulting in mesh sizes of 101,000, 202,000, and 304,000 elements, respectively. The results obtained using the 202,000 and 304,000 element meshes were comparable, with variations in maximum deformation not exceeding 2%. Therefore, considering the influence of calculation time and accuracy, the grid of 200,000 units can meet the calculation requirements, and the final grid division obtained is shown in Figure 2.

2.3. Initial Conditions and Simulation Analysis Methods

Due to the wheel hub being driven by bolts transmitted to bolt holes, five bolt holes and a mounting surface were chosen as fixed constraints. The applied loads and constraints on the wheel hub are illustrated in Figure 3. In the figure, the blue color is a fixed constraint. The loads on the wheel hub consist of three main components. Firstly, the support force acting uniformly distributed on the lower surface of the wheel hub’s rim seat in the π/3 arc region. The pressure was denoted as P₁ = 0.68 MPa. Considering the structural characteristics of the wheel spokes, the support force can be divided into two cases: one is directly acting on the wheel spoke (as shown in Figure 3a), and the other is acting on the wheel spoke ventilation opening (as shown in Figure 3b). Secondly, the tire pressure P₂ = 0.45 MPa acts on the wheel rim (as shown in Figure 3c). Lastly, the driving torque (torque on the wheel) T = 265 N·m transmitted from the engine acts on the bolt hole surface (as shown in Figure 3c). The fixed constraints imposed on the wheel hub are depicted in Figure 3d.

Based on the actual working conditions and loading requirements, the initial loads and boundary conditions for the wheel hub are set. This included applying loads, forces, or pressures on the wheel hub, as well as constraints and support methods. The material properties, such as elastic modulus, Poisson’s ratio, and density, were set based on the type and performance data of the wheel hub material. According to the static and modal analysis requirements, the appropriate solver is selected and the relevant parameters are configured. For the static analysis, the static analysis module in the ANSYS software was utilized to calculate the stress, strain, displacement, and other responses of the wheel hub under loading conditions. Depending on the requirements, the results for individual nodes and elements were obtained, and the post-processing and analysis of the results were performed. For the modal analysis, the appropriate type of modal analysis, such as natural frequency analysis, was selected. Similar to the static analysis, the material properties, such as elastic modulus, Poisson’s ratio, and density, were set. After selecting a suitable solver and applying corresponding boundary conditions and constraints, the modal analysis can be carried out to obtain the mode shape and natural frequency of each mode.

3. Results and Discussion

3.1. Static Analysis of the Wheel Hub

The static analysis of the wheel hub enables the determination of the deformation distribution under loading conditions. This helps in assessing the stiffness and deformation characteristics of the wheel hub, providing insights into the shape changes and magnitude of deformation under load. After applying the forces and constraints shown in Figure 3, the overall deformation result of the wheel hub is illustrated in Figure 4. Figure 4a represents the deformation result when the support force is acting directly on the wheel spoke. From the graph, it can be observed that under multiple loads and fixed constraints, the maximum displacement of the wheel hub is 0.30926 mm, with the maximum displacement occurring in the region near the inner side of the wheel hub where the support force is applied. The deformation at the connection between the wheel hub and the bolts was minimal. Figure 4b depicts the deformation result when the support force is acting on the ventilation opening. In this case, the maximum displacement of the wheel hub is 0.29096 mm, slightly smaller compared to the scenario with the support force acting on the wheel spoke, as shown in Figure 4a. Again, the maximum displacement occurred in the region near the inner side of the wheel hub where the support force was applied. Under the above two working conditions, the maximum displacement of the wheel hub is 0.30926 mm, less than 1 mm, which meets the design requirements of the automobile wheel hub. This indicates that the wheel hub structure design chosen in this study is reasonable and capable of meeting the requirements for automotive applications. The results of static analysis allowed for the identification of areas in the wheel hub that experience high stress and significant deformation. Based on this information, structural optimization can be performed, including adjusting the material distribution, enhancing the stiffness of high-stress regions, improving connection methods, and so on, in order to enhance the performance and quality of the wheel hub.

The equivalent stress of the wheel hub is shown in Figure 5. From Figure 5a, it can be observed that when the support force is acting directly on the wheel spoke, the maximum equivalent stress is 39.879 MPa, significantly lower than the yield strength of the selected material (205 MPa). The primary stress ranged from 4.4436 MPa to 26.591 MPa, distributed in a ring on the wheel rim near the point where the support force was applied, which falls within the safe range. As shown in Figure 5b, when the support force is acting on the ventilation opening, the maximum equivalent stress on the wheel hub is 45.946 MPa, still significantly lower than the yield strength of the selected material (205 MPa). The stress is within the safe range of 10.22 MPa and 30.635 MPa, and the rim is distributed in a ring near the support point. Based on the stress obtained for the wheel hub, the stress was mainly concentrated in the region near the applied force point on the wheel rim, particularly in the smaller fillet areas. Therefore, appropriately increasing the fillet radius can improve the stress distribution. By analyzing simulation results, the stress distribution in various parts of the wheel hub can be obtained, including the location of maximum stress and areas of stress concentration. This helps evaluate the strength and stability of the wheel hub under loading conditions.

3.2. Modal Analysis of the Wheel Hub

Based on the static analysis results of the wheel hub, a six-mode modal analysis was conducted. According to the distribution of the two positions of the supporting force on the wheel hub, the modal analysis is also divided into two cases.

Table 1. Comparison of modal frequencies for two different cases.

Modes Order	Frequency (Hz) (Support Force Acting on the Wheel Spoke)	Frequency (Hz) (Support Force Is Acting on the Ventilation Opening)
1	511.31	511.27
2	511.46	511.63
3	575.35	575.43
4	575.56	575.66
5	671.32	671.48
6	723.55	723.55

presents the modal analysis results for these two scenarios. After comparing the results, it was found that the mode analysis results were not significantly affected by the different support force conditions on the wheel hub. Therefore, for analysis purposes, the scenario with the support force acting on the ventilation opening can be selected. The results of the six-mode modal analysis for this scenario are shown in Figure 6. The colours are deformations. Red means the largest deformation and blue means the smallest. Figure 6a–f correspond to the six modes from Mode 1 to Mode 6, respectively. Modal analysis can be used to determine the natural frequencies of the wheel hub. These natural frequencies can be used to evaluate the response characteristics and stability of the wheel hub under different vibration modes.

Modal analysis results showed that the frequency values of the first four modes in the six modes are close to each other. Their mode shapes were also very similar, with only slight differences in certain vibration directions. Through the analysis of the mode shapes, it can be observed that there were primarily four types of mode shapes. The first type included Mode 1 and Mode 2, which exhibited predominantly vertical deformation vibrations. The second type included Mode 3 and Mode 4, where twisting deformation vibrations occurred in the wheel rim and spoke regions. The third type, represented by Mode 5, involved axial deformation vibrations of the wheel hub. The fourth type, represented by Mode 6, demonstrated triangular deformation vibrations in the wheel rim region as the mode order increases. Through the analysis of these modes, it can be seen that in order to extend the longevity of the wheel hub, the strength of the wheel rim and inner wheel spoke region should be appropriately reinforced; that is, the thickness of these positions should be increased.

External excitations on the wheel hub primarily include road surface excitation frequency, tire-induced imbalance excitation frequency, transmission system-induced imbalance excitation frequency, and engine vibration frequency. Based on engineering experience, road surface excitation frequencies are generally below 3 Hz for highways and well-maintained urban roads, while excitation frequencies for uneven road surfaces are generally below 11 Hz. For a typical gasoline engine passenger vehicle, the stable idle speed of a cold four-cylinder engine is usually between 1000 rpm and 1200 rpm. After the engine is warmed up, the idle speed typically ranges from 700 rpm to 800 rpm. Therefore, the vibration frequency of the engine at idle can be calculated to be between 23.33 Hz and 40 Hz. When a four-cylinder engine operates at a higher speed, such as 6000 rpm, the maximum vibration frequency of the engine can reach 200 Hz. Based on the above analysis, it can be concluded that the modal frequencies of the wheel hub are significantly higher than the external excitation frequencies. Based on the above analysis, it can be seen that this effectively avoids the occurrence of resonance phenomenon, which proves the rationality of wheel hub design. By comparing the natural frequencies of the wheel hub with the excitation frequencies from external sources, it was possible to determine whether resonance phenomena exist. Avoiding resonance is crucial in the design of the wheel hub to ensure its stability and reliability. Through the analysis of automotive wheel hub modal results, conclusions can be drawn regarding natural frequencies, mode shapes, mutual influences of vibration modes, and frequency responses. These conclusions are of great significance for improving wheel hub design, enhancing stability and reliability, as well as optimizing the dynamic performance of the wheel hub in practical use.

3.3. Optimization Design of the Wheel Hub

The optimization of wheel hub structure size adopted ANSYS software to realize parametric modeling and parameter optimization. By setting the corresponding range of input parameters, such as boundary conditions and initial conditions, the hub size parameters can be optimized. The input parameters were set to the rim thickness and spoke thickness, and the output parameters were set to the minimum safety factor, maximum mass, maximum deformation and maximum stress. The conditions were set with a minimum safety factor greater than 2 and a maximum deformation of less than 1 mm. The rim thickness range was set to 3–5 mm, and the spoke thickness range was set to 25–40 mm.

Based on the static analysis results for the wheel hub of a certain vehicle model, it was observed that the spokes of the wheel hub experience minimal stress, deformation, and almost zero strain. Therefore, this part exhibited sufficient strength and stiffness. By reducing the thickness of the spoke, increasing the area of ventilation openings, and removing the spoke material, the lightweight design goal can be achieved. These modifications not only served the purpose of ventilation but also reduced the weight of the wheel hub. Additionally, they enhanced the aesthetic appeal of the wheel hub to some extent. In locations where there was significant deformation and stress concentration, the thickness of the wheel hub and the fillets at the connections can be increased appropriately. Simultaneously, the thickness of other parts can be reduced to alter the stress distribution and reduce the weight of the wheel hub. Based on these optimization ideas, the preliminary optimized structure and approximate dimensions are shown in Figure 7. For example, the inner thickness of the rim was reduced to 6 mm, the corner radius of the ventilation opening was increased to 20 mm, and an elliptical ventilation hole with a major axis of 100 mm and a minor axis of 36 mm was created on the spoke.

For the optimized structure mentioned above, the deformation results at different loading positions are shown in Figure 8, and the corresponding equivalent stress results are shown in Figure 9. In Figure 8a and Figure 9a, the left subfigures represent the case where the support force is acting on the wheel spoke, while in Figure 8b and Figure 9b, the support force is acting on the ventilation opening. By comparing the force distribution in Figure 8 and Figure 9, it can be seen that the maximum deformation of the optimized hub is 0.40256 mm, and the stress distribution on the hub is more uniform than that before optimization. The maximum stress in the optimized wheel hub was 39.862 MPa, which was significantly lower than the yield strength of the material (205 MPa), indicating that the optimized wheel hub met the design requirements. The results of the modal analysis for modes 1 to 6 of the optimized wheel hub are shown in Figure 10a–f, respectively. According to the modal analysis results, the modal frequencies of the optimized wheel hub ranged from 366.39 Hz to 676.47 Hz, which was significantly different from the maximum external excitation frequency of 200 Hz, effectively avoiding resonance phenomena. Based on the comprehensive static and modal analysis results, it can be concluded that the optimized wheel hub meets the strength requirements, and its vibration frequencies are well separated from the external excitation frequencies. It is obvious that the maximum deformation of the optimized hub has increased, but the weight of the hub at this time is only 10.952 kg, which is about 15.6% lower than the weight of the non-optimized hub (12.979 kg). By optimizing the design of the hub, it is possible to improve the stability of a car during operation, which plays a crucial role in reducing air resistance and enhancing fuel efficiency.

3.4. Lightweight Analysis of the Wheel Hub

If the weight of the wheel hub is further reduced to achieve higher lightweight standards, it is difficult to achieve through structural optimization alone. In addition to optimizing the dimensions of the wheel hub to reduce material usage, another approach to further reduce the wheel hub’s weight is by replacing it with a lighter material. In this study, a magnesium alloy was selected as an alternative for the wheel hub, specifically the AZ31B alloy. It has a density of 1.74 g/cm³, elastic modulus of 45,000 MPa, Poisson’s ratio of 0.35, yield strength of 156 MPa, and compressive strength of 290 MPa. When the magnesium alloy is used as the wheel hub material, the deformation results are shown in Figure 11, and the corresponding equivalent stress results are shown in Figure 12, with the left subfigures representing the case where the support force is acting on the wheel spoke and the right subfigures representing the case where the support force is acting on the ventilation opening. The results of the modal analysis for each mode are shown in Figure 13.

From Figure 11 and Figure 12, it can be observed that the maximum deformation of the wheel hub is 0.71727 mm, which is less than 1 mm. It can also be seen from the figure that the maximum stress is 39.881 MPa, which is significantly lower than the yield strength of the material (156 MPa). The modal analysis results of the magnesium alloy wheel hub are shown in Figure 13. The modal frequencies of the optimized magnesium alloy wheel hub ranged from 339.95 Hz to 628.4 Hz, which was significantly different from the maximum external excitation frequency of 200 Hz, effectively avoiding resonance phenomena. The results of the static and modal analysis of the magnesium alloy wheel show that the design of the magnesium alloy wheel can meet the strength requirements. Moreover, the vibration frequency of the wheel hub is very different from the external excitation frequency, which can meet the vibration design requirements of the wheel hub. Additionally, for the same structure, the weight of the magnesium alloy wheel hub was 7.1105 kg, which was 35.1% lower than the weight of the aluminum alloy wheel hub (10.952 kg). This indicated that the use of lightweight materials through material substitution yields better results in terms of weight reduction compared to dimensional optimization. However, it is important to note that while the use of lightweight materials effectively reduces the weight of the wheel hub, it also increases the cost. Therefore, when designing and manufacturing wheels, it must not only fully consider the minimization of quality but also consider the overall economy of the wheels. Although lightweight design reduces the weight of vehicles, proper design can enhance vehicle safety performance by utilizing high-strength materials and optimizing structures. Automotive lightweight design can decrease the overall vehicle weight, thereby improving fuel efficiency and driving performance. The lighter vehicle weight also contributes to emission reduction and environmental friendliness.

4. Conclusions

This study focuses on the optimization design of automotive wheel hubs based on lightweight and economic considerations, conducting comprehensive research and optimization design of the wheel hub structure using finite element analysis. Taking into account the strength, vibration performance, and economic factors of the wheel hub, this study provides a feasible optimization design method for wheel hubs, serving as a valuable reference for the lightweight and performance enhancement of automotive wheel hubs. The main conclusions of this study are as follows:

(1)

The static analysis of the automotive wheel hub provided valuable insights into its structural response characteristics under different load conditions. It is obtained that increasing the fillet radius appropriately can improve the stress and displacement distribution.

(2)

The modal analysis results showed that the optimized wheel hub’s vibration frequencies were well separated from external excitation frequencies, indicating its excellent vibration performance and resonance avoidance.

(3)

The optimization design of the wheel hub led to improved strength and stiffness while reducing its mass. The deformation and stress distributions of the optimized wheel hub were obtained for various loading positions, demonstrating its improved performance. The stress is primarily concentrated near the load application points, particularly at the locations of smaller fillets. Therefore, appropriately increasing the fillet radius in that area can improve the distribution of stress. Although the maximum deformation of the optimized wheel hub has increased, the weight of the optimized wheel hub is 15.6% lower compared to the weight of the unoptimized wheel hub.

(4)

The lightweight analysis revealed that replacing the wheel hub material with a lightweight alloy, such as a magnesium alloy, further reduced its mass while maintaining the required strength and performance.

These findings contribute to the advancement of wheel hub optimization design and provide insights for the development of lightweight and high-performance automotive wheel hubs. Future research can explore additional lightweight materials and advanced optimization techniques to further enhance the wheel hub’s performance and efficiency.