Thermo-Mechanical Coupled Analysis of Electric Vehicle Drive Shafts

Abstract

With the growing concerns over global warming and abnormal weather patterns, the development of eco-friendly technologies has emerged as a critical research area in the transportation industry. In particular, the global automotive market, one of the most widely used sectors, has witnessed a surge in research on electric vehicles (EVs) in line with these trends. Compared to traditional internal combustion engine vehicles, EVs require components with high strength and durability to achieve optimal performance. This study focuses on the development of a constant velocity (CV) joint, a critical component for reliably transmitting the maximum output of an electric vehicle motor. Unlike conventional numerical methods, the proposed thermo-mechanical coupled analysis simultaneously accounts for thermal and mechanical interactions, providing more realistic operational performance predictions. This analysis, conducted using the thermal modules of Ls-Dyna and ANSYS Mechanical, effectively simulated field operation scenarios. Prototype testing under simulated conditions showed a 6% discrepancy compared to numerical predictions, validating the high accuracy and reliability of the proposed method. This robust thermo-mechanical coupled analysis is expected to improve the durability and reliability of CV joint designs, advancing electric vehicle component development.

1. Introduction

As concerns over climate change and the stability of energy resources continue to grow, there is a global surge in the demand for technologies that reduce carbon emissions and enable the development of sustainable transportation solutions. The automotive industry, in particular, significantly impacts global carbon emissions, underscoring the increasing importance of eco-friendly electric vehicles (EVs) that produce no exhaust emissions [1,2,3,4,5]. Compared to traditional internal combustion engine vehicles, EVs effectively mitigate negative environmental impacts while achieving continuous advancements across various domains through technological innovation. These advancements include improvements in charging speed, extended driving range, enhanced battery lifespan, and the development of high-performance components to ensure stable operation [6,7,8,9,10]. Such technological progress has garnered positive responses from both consumers and industries, leading to a steady increase in research and investment aimed at developing electric vehicles that combine reliability with high performance [10,11,12,13,14].

Electric vehicles (EVs) consist of key components such as electric motors, batteries, powertrains, and controllers. Among these, the electric motor converts electrical energy into rotational force, which is transmitted to the vehicle’s wheels through the powertrain to enable movement. The drive shaft, often referred to as the constant velocity (CV) joint, plays a crucial role by maintaining consistent rotational speed between the input and output shafts regardless of the steering angle. The CV joint directly influences the dynamic characteristics of EVs, as it must handle the high torque output delivered from the electric motor, which often fluctuates rapidly. This torque demand is significantly higher than that of traditional internal combustion engine vehicles. In large EVs, such as SUVs and pickup trucks, the CV joint must exhibit exceptional durability to maintain stable performance under heavy loads and harsh driving conditions, allowing for high-speed and long-distance driving. Increased loads can lead to friction and heat generation within the drive shaft, potentially altering its operational characteristics. An insufficient understanding of thermal phenomena may result in thermal deformation, increased friction and wear, and ultimately reduced durability, which can critically impact the safety and performance of the vehicle. Consequently, research on the design of drive shafts capable of withstanding such high-load environments is essential. However, validating performance through extensive prototype development and experimental testing is not only time- and cost-intensive but also faces limitations in directly observing internal components or evaluating the effects of various conditions. To overcome these challenges, the finite element method (FEM) has emerged as a vital tool for research and development [15,16,17,18,19,20]. The FEM enables the simulation of the complex structural behavior and physical phenomena occurring under diverse driving conditions in EVs. This approach allows for the analysis of structural and thermal stability during the design process, providing predictions of stress, deformation, and heat transfer. As a result, the FEM offers exceptional time and cost efficiency by enabling design optimization without the repeated need for prototype fabrication. Through precise numerical simulations, the FEM reduces dependency on physical testing, accelerating the development process while maintaining accuracy. This approach not only minimizes material and labor costs but also allows for the evaluation of multiple design scenarios under various conditions, ensuring optimal performance. By integrating the FEM into the design workflow, engineers can achieve faster iteration cycles and more reliable component development, making it a highly effective tool for modern engineering challenges.

2. Finite Element Method for CV Joint

In this study, the primary focus is on analyzing the CV joint, a critical component of the drive shaft in electric vehicles. The CV joint consists of multiple interconnected parts, resulting in a highly complex geometry and intricate operational mechanisms. The model used in this study, as illustrated in Figure 1, incorporates a novel joint design named the ball spline joint (BSJ), which combines a high-efficiency constant velocity (CV) joint with a ball spline structure capable of accommodating various angular movements [21]. To simulate the heat generated during the operation of this component, the analysis was conducted under the assumption that it rotates continuously at a fixed angle. The ball spline joint (BSJ) is designed to transmit power smoothly across a range of angles, from 0 degrees (straight-line driving) to 40 degrees (high-angle operation). Its design incorporates a ball spline structure in the center, allowing for seamless power transmission while accommodating suspension movements. However, for the purposes of this study, the ball spline movement was assumed to remain stationary to simplify the analysis. The BSJ comprises a power transmission joint section, consisting of an outer race, inner race, cage, and ball, as well as a ball spline shaft and a sleeve cage with balls. This integrated structure connects with the inner race of the CV joint, enabling the axial movement of the drive shaft and accommodating changes in vehicle ground clearance through the ball spline coupling mechanism. The BSJ transmits the rotational torque generated by the motor, during which the internal components undergo high-speed rotation. This operation induces friction among the internal components, leading to heat generation. Such thermal phenomena can cause a thermal deformation or expansion of the internal parts, resulting in the accumulation of internal stress. However, due to the geometric characteristics of the BSJ, directly observing the phenomena occurring within the joint during operation poses a significant challenge. In particular, the real-time observation or experimental validation of factors such as stress distribution changes, stress concentration, deformation, heat generation, and thermal stress during operation is highly constrained. Furthermore, as the BSJ is characterized by high-speed rotation and prolonged operation, performing long-term simulations of its real-world performance is inherently challenging.

In prior studies, quasi-static analysis has been employed to evaluate the contact forces and plastic deformation of constant velocity (CV) joint components for passenger vehicles [22]. However, quasi-static analysis is limited in its ability to account for time-dependent phenomena, as it evaluates systems under static conditions. This approach fails to adequately describe dynamic phenomena such as friction and plastic deformation arising from contact structures. To address these limitations, this study employs a combined approach using both Explicit and Implicit analysis methods to comprehensively simulate not only structural deformations during dynamic operation but also thermal interactions. The analyses were conducted using the Transient Thermal module of LS-Dyna and Ansys Mechanical. LS-Dyna is a software specialized in nonlinear finite element analysis, offering significant advantages in analyzing rapidly changing dynamic conditions through its Explicit analysis method [23,24,25,26]. Explicit analysis is particularly suited for physical phenomena that occur over short time spans, such as impacts, explosions, and collisions. It provides robust solutions for simulations involving nonlinearities and complex contact conditions, ensuring high stability even under challenging scenarios. Moreover, Explicit analysis excels in efficiently solving problems involving large deformations or multiple contact points, significantly reducing computation time while delivering reliable results. Due to these advantages, it is widely utilized across various industries, including automotive crash analysis, explosion studies in defense applications, and impact analysis [27,28,29,30,31,32,33,34].

Conversely, the thermal analysis capabilities of Ansys Mechanical employ an Implicit analysis method, which offers the advantage of delivering results efficiently even for extended simulation timeframes. Furthermore, it supports the application of diverse thermal boundary conditions, enabling more realistic and accurate analysis outcomes. These features make it particularly effective for analyzing structural deformations due to thermal expansion and evaluating thermal stress through integration with structural problems. In this study, LS-Dyna was utilized to simulate the initial short-term behavior and then calculate the temperature of critical components due to internal frictional stresses. Based on these results, a simulation procedure was established to predict nonlinear thermal phenomena and their locations during extended operation. To ensure the reliability of the analysis, temperature changes at measurable points identified in physical experiments were observed and compared with the simulation results for validation. The analytical process employed in this study is illustrated in Figure 2.

As shown in Figure 2, this study utilized ANSYS Workbench to establish the pre-processing framework for the analysis. Through this platform, a K-file containing the necessary information for the analysis was generated and formatted for compatibility with LS-Dyna. The K-file serves as an input data file that includes the geometric details of the analysis model, such as nodes and element information. Specifically, it contains the coordinates of nodes (spatial locations of each point) and the connectivity information of the elements, allowing the program to recognize the relationships between nodes. Additionally, the K-file incorporates various physical properties such as elastic modulus, density, and plastic deformation parameters, ensuring an accurate representation of real-world operating conditions. To conduct the dynamic analysis, the model defines initial conditions and external loading information, including friction coefficients, contact stiffness, and penetration tolerance, which characterize the contact interactions. This setup enables the simulation of complex physical interactions between components within the model.

In Solve Process 1, a thermo-structural coupled model in LS-Dyna was employed to perform dynamic analysis. Key results such as deformation, stress, and velocity were reviewed, with a particular focus on thermal analysis. In Solve Process 2, the thermal variations obtained from the LS-Dyna analysis were verified and incorporated into the Ansys Transient Thermal model for extended thermal analysis. The workflow of this study was designed as an integrated model linking LS-Dyna and Ansys Transient Thermal, ensuring that both analyses shared the same mesh elements. This setup enabled the mapping of results calculated in LS-Dyna onto the Thermal model, allowing for additional long-term thermal behavior analysis. In Solve Process 2, heat flux values at individual nodes, derived from the short-term dynamic analysis in LS-Dyna, were extracted and applied to the Ansys Transient Thermal model. Using this input, an extended thermal analysis was conducted to evaluate long-term behavior. The accuracy of the analysis was validated by comparing the simulation results with experimental data. The methodology proposed in this study enables an efficient thermo-structural coupled analysis of high-speed rotating components, contributing to improved design reliability under high-temperature and high-load environments.

2.1. Pre-Process

The geometry of the model used in the analysis is shown in Figure 3. The CV joint applied in this study, referred to as the ball spline joint (BSJ), was designed to maximize the structural advantages of the ball and ball spline mechanism. This design enables the BSJ to maintain performance even under high angular displacement conditions. To simulate harsh operating conditions, the physical phenomena occurring were modeled by setting the angle between the outer race and the shaft axis to 15° in a global coordinate system. This analysis was conducted to evaluate the structural stability and performance characteristics of the BSJ under extreme operating conditions.

To reduce computation time and focus on the region of interest, the power-transmitting shaft was modeled as a rigid body for the analysis. This shaft was configured with boundary conditions to transmit the torque generated by the motor. In contrast, other components were modeled as flexible bodies, allowing for the calculation of structural deformation and thermal changes. All components used in the analysis were assigned the material properties of AISI 4140, with the relevant properties specified in Table 1. Boundary conditions are summarized in Table 2. The outer race was set to rotate at 500 RPM, while a counteracting torque of 700 Nm was applied to the shaft, forming the loading conditions. Additional boundary conditions and key parameters are detailed in Table 2.

2.2. Solve Process 1 with Ls-Dyna

As previously noted, Explicit analysis using LS-DYNA often entails extensive computational time. Therefore, this study focuses on extracting essential thermal characteristics to optimize computational efficiency. Specifically, the dynamic behavior was analyzed for a duration of 0.36 s, corresponding to three rotations under a 500 RPM condition. The thermo-mechanical coupling equations employed in the analysis integrate the fundamental structural equations derived from Hooke’s law with the heat transfer equations. In this process, the thermal expansion of the material is modeled using the coefficient of thermal expansion (α), as shown in Equation (1):

(1)${\mathsf{\epsilon }}^{\mathrm{t}\mathrm{h}}=\mathsf{\alpha }\left(\mathrm{T}\right)\left(\mathrm{T}-{\mathrm{T}}_{\mathrm{r}\mathrm{e}\mathrm{f}}\right)$

The deformation due to thermal expansion calculated from Equation (1) is subsequently applied to the total strain calculation using Equation (2):

(2)$\left\{\mathsf{\epsilon }\right\}=\left\{{\mathsf{\epsilon }}^{\mathrm{t}\mathrm{h}}\right\}+{\left[\mathrm{D}\right]}^{-1}\left\{\mathsf{\sigma }\right\}$

Here, [D] represents the elasticity matrix of the material. At each element level, the strain is iteratively adjusted to maintain stress equilibrium with adjacent elements. This iterative process determines the stress and strain distribution within each component. Finally, the degrees of freedom associated with the dynamics and thermal properties of each component are computed and linked through the coupled governing equation shown below. The stress–strain relationship from Equation (2) is applied as the element load (F), ensuring convergence by accounting for material stiffness, thermal expansion, and heat transfer effects.

(3)$\left[\begin{array}{cc}\mathrm{M}& 0\\ 0& 0\end{array}\right]\left\{\begin{array}{c}\ddot{\mathrm{u}}\\ \ddot{\mathrm{T}}\end{array}\right\}+\left[\begin{array}{cc}\mathrm{C}& 0\\ 0& {\mathrm{C}}^{\mathrm{t}}\end{array}\right]\left\{\begin{array}{c}\dot{\mathrm{u}}\\ \dot{\mathrm{T}}\end{array}\right\}+\left[\begin{array}{cc}\mathrm{K}& {\mathrm{G}}^{\mathrm{T}}\\ \mathrm{G}& {\mathrm{K}}^{\mathrm{t}}\end{array}\right]\left\{\begin{array}{c}\mathrm{u}\\ \mathrm{T}\end{array}\right\}=\left\{\begin{array}{c}\mathrm{F}\\ \mathrm{Q}\end{array}\right\}$

• [M] = Element mass matrix;

• [C] = Element structural damping matrix;

• [K] = Element stiffness matrix;

• [G] = Thermal expansion matrix;

• {u} = Displacement vector;

• {F} = Combined element nodal force and pressure vectors;

• [C^t] = Element specific heat matrix;

• [K^t] = Element diffusion conductivity matrix;

• {T} = Temperature vector;

• {Q} = Combined element heat generation rate and convection surface heat flow vector.

This framework ensures the accurate simulation of the thermo-mechanical behavior of components by coupling the effects of displacement, stress, heat, and thermal expansion in a unified analysis.

Using these equations, it is possible to calculate structural deformation, heat generation, and deformation caused by thermal effects, allowing the precise simulation of the dynamic behavior of the system under external loads and temperature variations. The computation time for Explicit analysis using Ls-Dyna varies depending on factors such as geometry, mesh density, boundary conditions, and the computer specifications utilized. In this study, the analysis was conducted using Ls-Dyna in combination with Ls-PrePost 2024 R1 (4.11.0) software. The computations were performed on a system equipped with the following specifications: CPU: AMD Ryzen 9 5950X (16-Core), RAM: 128 GB, and GPU: NVIDIA GeForce GTX 1660 Super. The total computation time for the analysis amounted to 17 h, 26 min, and 40 s.

2.3. Solve Process 2 with Ansys Transient Thermal

Based on the average heat flux derived from Process 1, a thermal analysis was conducted using the Ansys Transient Thermal 2024 R1 program to predict the heat generation during the prolonged operation of the same model. As previously explained, constructing an analysis model that includes inter-component contact and deformation requires significant computational resources. To address this, it was assumed that the heat generated per rotation remained constant. Accordingly, the heat generation calculated in Process 1 was continuously applied to the friction surfaces in this analysis. The heat transfer from the surfaces was computed based on the governing equation shown in Equation (4). This analysis simulated the temperature variations over 120 s, corresponding to 2000 rotations at 500 RPM. To minimize discrepancies between simulations, the geometry and meshing were configured identically to those used in the previous analysis, and no positional displacements were considered. The thermal analysis was conducted using Fourier’s heat conduction equation as the governing equation, employing an Implicit analysis approach. This methodology enabled the prediction of thermal changes during prolonged rotations, providing results applicable to structural design optimization.

The governing equation used in the analysis is expressed as follows:

(4)$\mathsf{\rho }\mathrm{c}\left({\displaystyle \frac{\partial \mathrm{T}}{\partial \mathrm{t}}}+{\left\{\mathrm{v}\right\}}^{\mathrm{T}}\nabla \mathrm{T}\right)+\nabla ·\left\{\mathrm{q}\right\}=\ddot{\mathrm{q}}$

• ρ = Density;

• c = Specific heat;

• T = Temperature;

• t = Time;

• {v} = Velocity vector for the mass transport of heat;

• {q} = Heat flux vector;

• $\ddot{\mathrm{q}}$ = Heat generation rate per unit volume.

The simulation was performed under the same software and hardware specifications as those used in Process 1. By employing this approach, the thermal behavior of the system during extended operation was effectively predicted, yielding insights critical for structural design enhancements.

3. Results

The analysis was conducted following the previously described procedures and boundary conditions. This section summarizes the simulation results, validates each step of the methodology, and compares the outcomes with the experimental data to assess the proposed procedures’ accuracy and reliability. By systematically evaluating the results, this study ensures that the analytical approach aligns with real-world conditions and effectively predicts operational behaviors. The comparison with the experimental data serves to confirm the methodology’s validity, highlighting its robustness and practical value for analyzing complex thermal and mechanical interactions.

3.1. Results for Solve Process 1 with Ls-Dyna

To validate the accuracy of the analysis, the rotational speed was examined. Figure 4 illustrates the rotational velocity vectors, confirming that the outer race, cage, and inner race rotate at 500 RPM. This verifies that the applied rotational and loading conditions were appropriately implemented in the simulation. Based on the Explicit analysis results obtained from LS-Dyna, the stress distribution on individual components was further analyzed. The stresses in each part are the stresses generated by the delivery of the 700 Nm torque that was set as the load condition earlier. Figure 5 presents the stress distribution observed on the ball and cage. The analysis revealed that the maximum stress exerted on the cage was 354 MPa, corresponding to approximately 38% of the strength of the AISI 4140 material, indicating the effective utilization of the material’s capacity. Additionally, the maximum stress on the ball was calculated to be 200 MPa, with consistent patterns and trends observed across all eight balls. This uniform stress distribution indicates that all balls operate stably under evenly distributed loads, ensuring reliable performance.

The primary result obtained from Process 1 is the heat flux generated by friction between internal components. To quantify this, the heat flux values arising from friction between the key components of interest were calculated. The components under focus in this study include the inner race, ball, cage, and outer race. For each of these components, individual heat flux values were derived. Using the calculated heat flux values, the average heat flux acting on the contact surfaces was determined based on the nodes applied to the friction surfaces. The contact surfaces used for this analysis are illustrated in Figure 6, and the resulting heat flux values are summarized in Table 3. In addition, considering the situation of the verification experiment, the boundary condition was set to be convective heat transfer for the outer exposed surface as shown in Figure 6. The convective heat transfer coefficient on this surface is 15 W/m² °C, which assumes that the verification experiment is performed inside the chamber, so the surrounding air is stagnant and only the heat transfer of natural convection occurs.

3.2. Results for Solve Process 2 with Ansys Transient Thermal

Based on the heat flux derived from Process 1, a thermal analysis was conducted using ANSYS Transient Thermal to predict the temperature accumulation during prolonged operation. In real operating conditions, the ball continuously reciprocates along the grooves of the inner and outer races. Frictional heat is generated and transferred due to the contact between the ball and the cage surface designed to prevent the ball’s detachment. Additionally, boundary conditions were set to account for convective heat transfer on externally exposed surfaces, reflecting the conditions of the validation experiment. The convective heat transfer coefficient for these surfaces was set at 50 W/m² °C, assuming natural convection levels due to the stagnant air environment within the experimental chamber. However, accurately simulating prolonged operational phenomena significantly increases computational complexity and cost, presenting practical challenges. To address this, this study assumes that a uniform heat flux is applied across the entire contact area between the ball and the respective components. This assumption reflects the high-speed movement of the ball and the grease-filled interior that facilitates the smooth operation and uniform heating of the components. This approach aims to enhance the efficiency of the long-term analysis by simplifying the complex heat transfer phenomena. The application of the heat flux to key contact areas, as illustrated in Figure 6, effectively simulates the impact of heat flux on major contact surfaces, providing a streamlined yet accurate representation of thermal behavior.

3.3. Results After Processes 1 and 2

The results derived from Process 1 and Process 2 are presented in Figure 7, which illustrates the temperature distribution across all components after 120 s of operation. The analysis revealed that the cage region maintains the highest temperature due to heat transfer from frictional interactions. This finding indicates that the cage serves as the primary heat accumulation point during operation, emphasizing its critical role in the system’s thermal behavior. The thermal properties of the cage can significantly influence the overall performance and durability of the system, highlighting the importance of optimizing this component to ensure reliable operation under prolonged and high-load conditions.

3.4. Experimetal Validation

To validate the simulation results, external temperature measurements were conducted using a test setup as shown in Figure 8. The experiments utilized the Drive Shaft Vibration Performance Tester (TSK, Tochigi, Japan), with the test samples subjected to specified conditions: a torque of 700 Nm and a rotational speed of 500 RPM at the designated angular displacement. Two temperature measurement methods were applied during the rotation of the samples. First, a non-contact laser thermometer (BS-05T, OPTEX, Otsu, Japan) was used to measure the temperature. Second, a thermal imaging camera (FLIR E8 XT, FLIR, Wilsonville, OR, USA) was employed to simultaneously record the temperature at the center of the external joint on the outer race of the BSJ, where temperature changes were accessible for monitoring. The measurements, which are summarized in Table 4, reveal a discrepancy of approximately 6% between the experimental and simulated values, validating the accuracy and reliability of the proposed analytical procedure and methodology. This result demonstrates that the simulation approach effectively captures the thermal behavior of the system under the given operating conditions.

4. Conclusions

This study presents a novel approach to analyzing and optimizing the design of constant velocity joints (CV joints), a critical component of electric vehicle drive shafts, under high-load and high-speed rotation conditions. By performing thermo-structural coupled analysis, the research aimed to evaluate the thermal and structural changes that occur during operation and support design optimization. The study utilized LS-Dyna for dynamic simulations and Ansys Transient Thermal for modeling thermal behavior. This dual-software approach enabled the efficient analysis of heat generation due to friction during high-speed rotation and the resulting structural stress distribution. The key takeaways from the study are as follows:

• The proposed methodology consisted of two primary stages. In the first stage, LS-Dyna was employed to perform short-term dynamic analysis and calculate heat flux resulting from friction between the internal components of the CV joint. In the second stage, Ansys Transient Thermal used the derived heat flux data to simulate the long-term temperature distribution and thermal effects under operational conditions.

• The integration of these tools facilitated the prediction of thermal behavior and structural deformation in environments resembling actual operating conditions. The analysis revealed the temperature and stress distributions across key components, including the ball, cage, and outer race, with the cage exhibiting the highest temperature.

• Experimental validation showed that the discrepancy between simulated and measured data was within 6%, confirming the reliability of the proposed methodology.

• These findings demonstrate the effectiveness of the proposed simulation-driven design tool in evaluating the performance of drive shafts under high-speed and high-load conditions. By eliminating the need for repetitive prototyping, the methodology offers significant potential for reducing development time and cost in electric vehicle component design.

• However, this study has limitations, such as the inability to fully account for all detailed contact conditions.

• Future research incorporating diverse operating conditions and more complex friction models is necessary. Such advancements are expected to further enhance the design reliability and durability of electric vehicle drive shafts.

Author Contributions

Conceptualization, S.-E.K., J.-L.P. and Y.J.; methodology, C.-H.J., M.-G.L. and Y.J.; software, S.-E.K. and C.-H.J.; validation, S.-E.K. and S.H.; investigation, S.-E.K. and S.H.; writing—original draft preparation, S.-E.K. and C.-H.J.; writing—review and editing, S.-E.K., C.-H.J., S.H. and Y.J.; supervision, M.-G.L. and Y.J.; funding acquisition, J.-L.P. and Y.J. All authors have read and agreed to the published version of the manuscript.

Institutional Review Board Statement

Not applicable.

Informed Consent Statement

Not applicable.

Data Availability Statement

The data presented in this study are available at the request of the corresponding author. The data are not publicly available due to the copyright of the company.

Conflicts of Interest

The authors declare no conflict of interest.

Footnotes

Disclaimer/Publisher’s Note: The statements, opinions and data contained in all publications are solely those of the individual author(s) and contributor(s) and not of MDPI and/or the editor(s). MDPI and/or the editor(s) disclaim responsibility for any injury to people or property resulting from any ideas, methods, instructions or products referred to in the content.

Figures and Tables

Figure 1. Schematic of ball spline joint.

Figure 2. Proposed methodology.

Figure 3. Angle of joint.

Figure 4. Velocity vector. (a) Schematic of velocity vector. (b) Rotational speed.

Figure 5. Resultant stress. (a) Stress of cage. (b) Effective stress of ball.

Figure 6. Heat flux on parts. (a) Heat flux on outer race groove. (b) Heat flux on inner race groove. (c) Heat flux on cage. (d) Heat flux on ball.

Figure 7. Resultant temperature. (a) Resultant temperature of all parts. (b) Resultant temperature of outer race. (c) Resultant temperature of cage wall. (d) Resultant temperature of ball.

Figure 8. Experimental validation apparatus.

Table 1

Mechanical properties for AISI 4140.

Property	Value	Unit
Density	7.85	$\mathrm{g}/{\mathrm{c}\mathrm{m}}^3$
Young’s Modulus	205	$\mathrm{G}\mathrm{P}\mathrm{a}$
Yield Stress	785	$\mathrm{M}\mathrm{P}\mathrm{a}$
Poisson’s Ratio	0.29
$\mathrm{Thermal} \mathrm{Expansion} \mathrm{Coefficient} (0–100 °\mathrm{C}$)	12.2	$\mathsf{\mu }\mathrm{m}/\mathrm{m}\mathrm{℃}$
Thermal Conductivity (100 °C)	42.6	$\mathrm{W}/\mathrm{m}\mathrm{K}$

Table 2

Process conditions.

Parameter	Value	Unit
Initial temperature	28	°C
Initial angular velocity	500	$\mathrm{R}\mathrm{P}\mathrm{M}$
Torque	700	$\mathrm{N}·\mathrm{m}$
Static friction coefficient	0.1
Dynamic friction coefficient	0.06
Total analysis time	300	$\mathrm{s}$

Table 4

Temperature comparisons among sensors and simulation.

Source	Value [°C]	Error Rate [%]
Simulation	61.09
Non-Contact sensor	65.24	6.37
Thermal Imaging Camera	64.7	5.59

Table 3

Calculated heat flux.

Parts	Heat Flux (w/m2)
	Outer Race	Inner Race	Cage	Ball
A	3410	6250	15,600	6320
B	5100	6710	8770	6970
C	4990	8820	12,800	7790
D	4240	7910		7650
E	4940	7330		8200
F	2930	4600		8100
G	3570	6140		8860
	3690	6850		7230

References

1. Uraoka, T.; Parra-Blanco, A.; Yahagi, N. Colorectal Endoscopic Submucosal Dissection: Is It Suitable in Western Countries?. J. Gastroenterol. Hepatol.; 2013; 28, pp. 406-414. [DOI: https://dx.doi.org/10.1111/jgh.12099] [PubMed: https://www.ncbi.nlm.nih.gov/pubmed/23278302]

2. Sun, X.; Li, Z.; Wang, X.; Li, C. Technology Development of Electric Vehicles: A Review. Energies; 2020; 13, 90. [DOI: https://dx.doi.org/10.3390/en13010090]

3. Liu, X.; Zhao, F.; Hao, H.; Liu, Z. Opportunities, Challenges, and Strategies for Developing Electric Vehicle Energy Storage Systems under the Carbon Neutrality Goal. World Electr. Veh. J.; 2023; 14, 170. [DOI: https://dx.doi.org/10.3390/wevj14070170]

4. Ghosh, A. Possibilities and Challenges for the Inclusion of the Electric Vehicle (EV) to Reduce the Carbon Footprint in the Transport Sector: A Review. Energies; 2020; 13, 2602. [DOI: https://dx.doi.org/10.3390/en13102602]

5. Wang, M.; Wang, Y.; Chen, L.; Yang, Y.; Li, X. Carbon Emission of Energy Consumption of the Electric Vehicle Development Scenario. Environ. Sci. Pollut. Res.; 2021; 28, pp. 42401-42413. [DOI: https://dx.doi.org/10.1007/s11356-021-13632-z]

6. Husain, I.; Ozpineci, B.; Islam, M.S.; Gurpinar, E.; Su, G.-J.; Yu, W.; Chowdhury, S.; Xue, L.; Rahman, D.; Sahu, R. Electric Drive Technology Trends, Challenges, and Opportunities for Future Electric Vehicles. Proc. IEEE; 2021; 109, pp. 1039-1059. [DOI: https://dx.doi.org/10.1109/JPROC.2020.3046112]

7. Zakaria, H.; Hamid, M.; Abdellatif, E.M.; Imane, A. Recent Advancements and Developments for Electric Vehicle Technology. Proceedings of the 2019 International Conference of Computer Science and Renewable Energies (ICCSRE); Agadir, Morocco, 22–24 July 2019; pp. 1-6. [DOI: https://dx.doi.org/10.1109/ICCSRE.2019.8807726]

8. Lebrouhi, B.E.; Khattari, Y.; Lamrani, B.; Maaroufi, M.; Zeraouli, Y.; Kousksou, T. Key Challenges for a Large-Scale Development of Battery Electric Vehicles: A Comprehensive Review. J. Energy Storage; 2021; 44, 103273. [DOI: https://dx.doi.org/10.1016/j.est.2021.103273]

9. Kumar, M.S.; Revankar, S.T. Development Scheme and Key Technology of an Electric Vehicle: An Overview. Renew. Sustain. Energy Rev.; 2017; 70, pp. 1266-1285. [DOI: https://dx.doi.org/10.1016/j.rser.2016.12.027]

10. Matanov, N.; Zahov, A. Developments and Challenges for Electric Vehicle Charging Infrastructure. Proceedings of the 2020 12th Electrical Engineering Faculty Conference (BulEF 2020); Varna, Bulgaria, 9–12 September 2020; [DOI: https://dx.doi.org/10.1109/bulef51036.2020.9326080]

11. Mazali, I.I.; Daud, Z.H.C.; Hamid, M.K.A.; Tan, V.; Samin, P.M.; Jubair, A.; Ibrahim, K.A.; Kob, M.S.C.; Wang, X.; Talib, M.H.A. Review of the Methods to Optimize Power Flow in Electric Vehicle Powertrains for Efficiency and Driving Performance. Appl. Sci.; 2022; 12, 1735. [DOI: https://dx.doi.org/10.3390/app12031735]

12. Cai, W.; Wu, X.; Zhou, M.; Liang, Y.; Wang, Y. Review and Development of Electric Motor Systems and Electric Powertrains for New Energy Vehicles. Automot. Innov.; 2021; 4, pp. 3-22. [DOI: https://dx.doi.org/10.1007/s42154-021-00139-z]

13. Fodorean, D. Study of a High-Speed Motorization with Improved Performances Dedicated for an Electric Vehicle. IEEE Trans. Magn.; 2014; 50, pp. 921-924. [DOI: https://dx.doi.org/10.1109/TMAG.2013.2279240]

14. Bayar, K.; Wang, J.; Rizzoni, G. Development of a Vehicle Stability Control Strategy for a Hybrid Electric Vehicle Equipped with Axle Motors. Proc. Inst. Mech. Eng. Part D J. Automob. Eng.; 2012; 226, pp. 795-814. [DOI: https://dx.doi.org/10.1177/0954407011433396]

15. Horváth, K.; Zelei, A. Simulating Noise, Vibration, and Harshness Advances in Electric Vehicle Powertrains: Strategies and Challenges. World Electr. Veh. J.; 2024; 15, 367. [DOI: https://dx.doi.org/10.3390/wevj15080367]

16. Ling, C.; Wang, L.; Kan, C.-D.; Yang, C. Thermal–Electrical–Mechanical Coupled Finite Element Models for Battery Electric Vehicle. Machines; 2024; 12, 596. [DOI: https://dx.doi.org/10.3390/machines12090596]

17. Anggara, H.D. Revitalizing Vehicle Innovation: Exploring Electric Car Chassis Structures through Finite Element Analysis. Innov. Eng.; 2024; 1, pp. 50-59. [DOI: https://dx.doi.org/10.58712/ie.v1i1.6]

18. Kant, K. Finite Element Simulation Based Design and Optimization of Electric Motors for EV/HEV Traction Application. Massachusetts Institute of Technology. 1970; Available online: https://hdl.handle.net/1721.1/122551 (accessed on 1 October 2024).

19. Bonanno, F.; Capizzi, G.; Coco, S.; Laudani, A.; Sciuto, G.L. A Coupled Design Optimization Methodology for Li-Ion Batteries in Electric Vehicle Applications Based on FEM and Neural Networks. Proceedings of the 2014 International Symposium on Power Electronics, Electrical Drives, Automation and Motion; Ischia, Italy, 18–20 June 2014; [DOI: https://dx.doi.org/10.1109/speedam.2014.6872017]

20. Booncherdchoo, C. Electric Vehicle Structure Analysis Using Finite Element Method (FEM). Intellectual Repository at Rajamangala University of Technology Phra Nakhon. 2018; Available online: http://repository.rmutp.ac.th/handle/123456789/2661 (accessed on 1 October 2024).

21. Park, J.C. Variable Shaft with a Ball Spline and Constant Velocity Joint Assembly. Republic of Korea Patent; No. 10-2169726, 23 October 2020; [DOI: https://dx.doi.org/10.8080/1020190118515]

22. Yan, S.; Kong, Z.; Liu, H.; Zhang, L.; Hu, X.; Hou, Y. Power Loss Evaluation of an E-Axle Gearbox Considering the Influence of Gear Oil Factors. Lubricants; 2024; 12, 11. [DOI: https://dx.doi.org/10.3390/lubricants12010011]

23. Liu, Y. ANSYS and LS-Dyna Used for Structural Analysis. Int. J. Comput. Aided Eng. Technol.; 2008; 1, 31. [DOI: https://dx.doi.org/10.1504/IJCAET.2008.021254]

24. Elmarakbi, A.M.; Hu, N.; Fukunaga, H. Finite Element Simulation of Delamination Growth in Composite Materials Using LS-Dyna. Compos. Sci. Technol.; 2009; 69, pp. 2383-2391. [DOI: https://dx.doi.org/10.1016/j.compscitech.2009.01.036]

25. Rabiee, A.; Ghasemnejad, H. Finite Element Modelling Approach for Progressive Crushing of Composite Tubular Absorbers in LS-DYNA: Review and Findings. J. Compos. Sci.; 2022; 6, 11. [DOI: https://dx.doi.org/10.3390/jcs6010011]

26. Song, M.; Tong, Z.; Yuan, W.; Tian, B. A Numerical Simulation Method for Prediction of Ice Resistance and Ship Motion in Level Ice. Proceedings of the ASME 2024 43rd International Conference on Ocean, Offshore and Arctic Engineering; Singapore, 9–14 June 2024; V006T07A013 [DOI: https://dx.doi.org/10.1115/OMAE2024-123950]

27. Felaco, A.; Opran, C.G.; Lamanna, G. Numerical Analysis Techniques for Studying the Structural Strength of a Vehicle in Terms of Absorbed Energy. Macromol. Symp.; 2024; 413, 3. [DOI: https://dx.doi.org/10.1002/masy.202400050]

28. Droździel, P.; Pasaulis, T.; Pečeliūnas, R.; Pukalskas, S. Evaluation of the Energy Equivalent Speed of Car Damage Using a Finite Element Model. Vehicles; 2024; 6, pp. 632-650. [DOI: https://dx.doi.org/10.3390/vehicles6020029]

29. Yin, Z.F.; Yu, S.Z.; Ma, B.; Sun, Y.L. Corrosion Evaluation and Mechanical Life Prediction of J55 Tubing Steel under Air-Foam Flooding Oil Well Conditions. J. Mater. Eng. Perform.; 2024; [DOI: https://dx.doi.org/10.1007/s11665-024-09780-1]

30. Muresanu, A.D.; Dudescu, M.C. Modelling of a Cylindrical Battery Mechanical Behavior under Compression Load. Batteries; 2024; 10, 353. [DOI: https://dx.doi.org/10.3390/batteries10100353]

31. Kaushik, A.; Rabiei, A. An Interactive Fluid–Solid Approach for Numerical Modeling of Composite Metal Foam Behavior under Compression. Adv. Eng. Mater.; 2024; [DOI: https://dx.doi.org/10.1002/adem.202401267]

32. Demiyanushko, I.V.; Lokit, A.G.; Mikheev, P.S.; Titov, O.V. Digital Modelling of Trailer Truck Mounted Attenuator and Its Reliability Evaluation. Advances in Asian Mechanism and Machine Science; Tuleshov, A.; Jomartov, A.; Ceccarelli, M. Mechanisms and Machine Science Springer: Cham, Switzerland, 2024; Volume 167, pp. 1-34. [DOI: https://dx.doi.org/10.1007/978-3-031-67569-0_34]

33. Pavlovic, A.; Minak, G. Numerical Investigation of Low-Velocity Ice Impact on a Composite Ship Hull Using an FEM/SPH Formulation. Appl. Sci.; 2024; 14, 7679. [DOI: https://dx.doi.org/10.3390/app14177679]

34. Karpik, A.; Cosco, F.; Mundo, D. Dynamic Error Estimation in Higher-Order Finite Elements. Designs; 2024; 8, 79. [DOI: https://dx.doi.org/10.3390/designs8040079]