Finite Element Analysis and Optimization of Hydrogen Fuel Cell City Bus Body Frame Structure

Abstract

Hydrogen fuel cell city bus is a type of new energy public transportation. In this paper, in order to evaluate the safety performance of a newly developed hydrogen fuel cell city bus body frame designed by the collaborating enterprise, finite element analysis is conducted to investigate its structural mechanics and dynamic characteristics under four typical operating conditions, including horizontal bending, ultimate torsion, emergency cornering, and emergency braking. Based on the simulation results, although the body frame of the bus meets the stiffness design requirements and avoids body resonance, it exhibits maximum stresses of 328.9 MPa and 348.6 MPa under emergency cornering and ultimate torsion conditions, respectively, exceeding the material yield strength and failing to satisfy the strength design requirements. Therefore, the size optimization method is employed to optimize the thickness of the body frame components. After optimization, the maximum stresses are reduced to 262.7 MPa and 300.6 MPa, respectively, representing a reduction of up to 20.13%. The optimization significantly improves performance and meets the strength design requirements. Furthermore, the body frame is lightened by 106 kg, achieving the goal of weight reduction.

1. Introduction

The bus provides a convenient mode of transportation, solves traffic congestion, reduces transportation costs, minimizes environmental pollution, and promotes interconnection between urban and rural areas. It is an indispensable public transportation vehicle in daily life. Under the background of advocating for low-carbon alternatives and environmental protection in the world, the hydrogen fuel cell bus has been actively promoted by society with its characteristics of energy saving and emission reduction [1,2,3]. Due to its environmental friendliness, sustainability, long-range, rapid charging, and powerful performance, the hydrogen fuel cell bus has gained favor from numerous countries and automotive companies [4,5,6,7]. However, compared to traditional fuel-powered bus, the hydrogen fuel cell city bus is equipped with additional systems, such as hydrogen storage, power batteries, and fuel cell systems, causing significant changes in the load distribution of the bus body frame [8,9,10]. Therefore, it is essential to conduct safety analyses of the static and dynamic characteristics of the bus body frame under typical operating conditions [11,12].

Safety analysis of the automobile body is commonly conducted using the finite element method, which enables the shortening of the vehicle’s development time during the early stages of automotive product research. Additionally, it facilitates subsequent improvements and adjustments, significantly reducing the development costs of vehicles [13,14,15,16]. Zhu J et al. established a finite element model of the bus body and conducted a dynamic modal analysis to obtain its eigenvalues and mode shapes [17]. Peng S H et al. conducted a modal analysis to verify the dynamic performance of the body frame [18]. Shen Y F et al. conducted a static analysis to investigate the strength and modal characteristics of the bus body frame [19]. Chen Y H et al., conducted a safety analysis of the strength and stiffness of the bus body frame by performing static finite element simulations based on the established bus model [20].

Performing static finite element analysis on the bus body frame allows us to obtain its maximum stress values, stress concentration locations, and maximum displacement values, which reflect the static structural mechanical performance of the bus body frame, including its strength and stiffness characteristics [21,22,23]. Performing dynamic modal analysis on the bus body frame allows us to obtain its natural frequencies and mode shapes, which reflect its dynamic performance, evaluate the body’s connection conditions, and identify the possibility of body resonance [24,25]. Therefore, an increasing number of researchers have adopted static and modal analysis methods to verify the safety of bus body frame structures. In this paper, the strength and stiffness performance of the hydrogen fuel cell city bus body frame are examined through static finite element simulations. Additionally, the dynamic characteristics of the body frame are analyzed for safety through modal simulation tests.

When the vehicle body does not meet safety requirements or requires lightweighting due to excessive safety margins, it is common to achieve the desired objectives by either optimizing the body structure or replacing it with high-strength lightweight materials [24,25,26,27]. Wei Z L et al., conducted a topology optimization of the bus body frame based on its stress characteristics, thereby enhancing the strength and stiffness of the body frame [28]. Fu C L et al., conducted a lightweight design of electric buses by optimizing the dimensions of the electric bus structure, thus improving the electric bus’s driving range [29]. Jilek P et al. conducted a strength analysis of automobile beams using the finite element method and subsequently achieved the goal of improving their strength and reducing weight by applying high-strength materials [30]. The hydrogen fuel cell city bus studied in this paper is a large and complex assembly, with the bus body frame being composed of numerous welded rods, requiring high assembly accuracy. Therefore, the approach of size optimization is adopted to enhance its strength and stiffness characteristics, thereby meeting the design requirements of the bus body frame.

As a new energy public transportation vehicle, hydrogen fuel cell city buses are widely used throughout the country. To ensure the driving safety of the studied hydrogen fuel cell city bus, this paper primarily adopts the finite element simulation method to investigate its mechanical performance. Firstly, a finite element model of the hydrogen fuel cell city bus body is established. Subsequently, static finite element simulations and dynamic modal simulations are conducted under four typical operating conditions to study its strength, stiffness, and dynamic characteristics. The simulation results are analyzed comprehensively. In cases where the mechanical performance of the hydrogen fuel cell city bus body does not meet the design requirements, a size optimization approach is employed to optimize the body frame. The optimized bus body frame is then validated through simulation tests, ultimately achieving the objective of ensuring the safe operation of the hydrogen fuel cell city bus.

2. Model Establishment and Simulation Test Design

2.1. Establishment of Finite Element Model

2.1.1. Bus Parameters

In response to the call for energy conservation, emission reduction, and environmental protection, the collaborative enterprise in this paper developed a new type of hydrogen fuel cell city bus. This paper verifies the safety performance of the hydrogen fuel cell city bus body frame through finite element simulation tests. The body frame of the hydrogen fuel cell city bus is a fully load-bearing structure, and the physical drawing of the bus is shown in Figure 1. The overall dimensions of the bus are 10,500 mm × 2500 mm × 3390 mm, with a wheelbase of 5100 mm, and the entire bus body frame adopts a full load-bearing structure. The hydrogen fuel cell city bus employs a hybrid drive system with two types of batteries for propulsion. Under normal driving conditions, the hydrogen fuel cell serves as the sole power source. During acceleration, the power battery provides additional power support. During braking or idle conditions, the power battery absorbs the excess output energy from the hydrogen fuel cell and stores it for later use.

2.1.2. Mesh and Materials

According to the actual size of the dimensional parameters of the hydrogen fuel cell city bus, the bus body frame is modeled in 3D in NX 10.0 software (Siemens PLM Software, Plano, TX, USA). The 3D model file is imported into HyperMesh 2017 (Altair, Troy, MI, USA,) for finite element modeling, and then the OptiStruct software 2018 (Altair, Troy, MI, USA) is used for simulation tests. Due to the numerous components and complex structure of the hydrogen fuel cell bus body frame, appropriate simplifications are required during the modeling process to improve modeling efficiency. Non-load-bearing components that do not affect the simulation results are simplified or omitted from the model.

The body frame of this particular bus model is primarily composed of thin-walled structural components, where the length and width of these components are much larger than their thickness. To model the thin-walled structure efficiently, mid-surface extraction is adopted, and the relevant mid-surfaces are then meshed. Due to the advantages of fast computation speed and stable solutions, the mesh type chosen is quadrilateral shell elements with a mesh size of 10 mm [31]. After dividing the bus body frame into meshes, the total number of shell elements is 1,028,691, among which triangular elements account for 0.33% of the total shell elements, with a count of 3294. This indicates that the mesh quality of the bus body frame is relatively good.

When establishing the finite element model of the bus body frame, it is essential to consider both the connection relationships between components and their material properties. The body frame of this hydrogen fuel cell city bus is primarily assembled from different types of structural components, and welding is used as the connecting method. The material of the body frame studied in this paper is Q345 steel, and specific parameters for material assignment to various components of the body frame are shown in

Table 1. Material properties of Q345.

Materials	Density	Elasticity Modulus	Poisson’s Ration	Yield Strength
Q345	7850 kg/m3	206,000 MPa	0.3	345 MPa

.

2.1.3. Load Handling

For a fully load-bearing hydrogen fuel cell city bus, there are four typical working conditions during its daily operation. These conditions include horizontal bending, ultimate torsion, emergency braking, and emergency cornering [32].

The overall structure of the hydrogen fuel cell city bus studied in this paper is relatively complex. To better simulate the real-life load distribution of the bus, other additional loads attached to the bus are applied to the corresponding assemblies and positions through concentrated loads. The load on the hydrogen fuel cell city bus body frame mainly includes the hydrogen fuel cell system, hydrogen storage system, power battery, seats, air conditioning, passengers, etc. The bus is calculated to have 20 seats and 39 passengers, where each seat is 11 kg and each passenger averages 65 kg. The weight distribution of the main load is shown in

Table 2. Main mass parameters of the hydrogen fuel cell city bus.

Name	Quality/kg
Hydrogen storage system	480
refrigeration	330
Power Battery Pack	400
Fuel Cell System	174
Seat	220
Passengers	2535

.

After the weight distribution is completed, the final simplified finite element model of the bus body frame is shown in Figure 2.

2.2. Design of Static Structural Mechanics Simulation Tests

2.2.1. Horizontal Bending Condition

Horizontal bending is one of the most common operating conditions for buses. In this condition, the bus simulates uniform-speed driving or being stationary on a level road with all four wheels in contact with the ground, the bus body frame bends around the X-axis in the longitudinal direction of the bus. The body frame of the bus is only subjected to its own weight and the load from the passengers. For this condition, boundary conditions are set to constrain the translational degrees of freedom in the X, Y, and Z directions for the front wheels while constraining only the translational degree of freedom in the Z direction for the rear wheels, with the other degrees of freedom being released.

2.2.2. Ultimate Torsion Condition

Ultimate torsion is a condition in which the bus experiences asymmetric loading during its operation. It is the most critical torsion load in the classical driving conditions because the ultimate torsional condition is to test the maximum torque or moment that the bus body frame can withstand in the torsional direction. It simulates a scenario where one wheel of the bus is lifted when driving over uneven road surfaces, leading to a twisting state of the bus. As the hydrogen fuel cell city bus is equipped with a hydrogen storage system at the front, there is a possibility of a forward weight shift. Hence, in this study, the right front wheel of the bus is selected to be lifted. The boundary conditions are set to constrain the translational degrees of freedom in the Y and Z directions for the left front wheel, constrain the translational degrees of freedom in the X, Y, and Z directions for the left rear wheel, constrain the translational degrees of freedom in the X and Z directions for the right rear wheel, and release all degrees of freedom for the right front wheel.

2.2.3. Emergency Braking Condition

When buses are driving on urban roads, emergency braking situations frequently occur due to various road conditions. During emergency braking, the bus body frame not only bears its existing load but also experiences a significant inertial force acting forward. Under full load and emergency braking conditions, this study focuses on the impact of inertial forces on the hydrogen fuel cell city bus body frame during maximum deceleration with the maximum braking force applied. In the simulation process of the emergency braking condition, the bus body frame is subjected to a simulated acceleration of 0.8 g in the X-axis direction [33]. The boundary conditions were set as follows: the front wheels were constrained in the X-, Y-, and Z-direction translational degrees of freedom, the rear wheels were constrained in the Z-direction translational degree of freedom, and all other degrees of freedom were released.

2.2.4. Emergency Cornering Condition

The emergency cornering condition mainly simulates the situation when the bus needs to make an emergency turn during its operation. When the hydrogen fuel cell city bus performs an emergency turn, the body frame is subjected not only to its own weight but also to the centrifugal force in the opposite direction of the turn, resulting in a lateral force acting on the overall body. When the lateral acceleration exceeds a certain value, there is even a risk of rollover, making emergency cornering a highly dangerous condition. In the simulation analysis of this condition, a Y-axis 0.3 g lateral acceleration is applied to the entire bus to simulate the loading condition during an emergency right turn [32]. The boundary conditions are set as follows: the left front wheel’s Z-direction translational degree of freedom is constrained, the right front wheel’s Y and Z-direction translational degrees of freedom are constrained, the left rear wheel’s X and Z-direction translational degrees of freedom are constrained, and the right rear wheel’s X, Y, and Z-direction translational degrees of freedom are constrained.

2.3. Design of Dynamic Modal Simulation Tests

Dynamic modal analysis is a fundamental method for assessing the dynamic characteristics of vehicles. Modal analysis can be categorized into two types: free modal analysis and constrained modal analysis [34]. The free modal analysis involves studying the vibration characteristics of the bus body frame without considering the effects of external loads, where the analysis is focused on the bus’s completely unconstrained vibration behavior. On the other hand, the constrained modal analysis refers to the determination of vibration characteristics under actual operating conditions, considering the influence of applied loads on the bus body frame.

Firstly, due to the complexity of the hydrogen fuel cell bus body frame with numerous components and intricate connections, modal analysis is of paramount importance for the established finite element model. Through modal analysis, the overall connectivity of the bus body frame can be visually assessed. Secondly, during city bus operations, the bus is subjected to various excitations from both internal and external sources, with the most common being road surface excitations caused by different road conditions. Modal analysis helps determine whether the natural frequencies of the bus body coincide with these excitations. Once resonance occurs, it can lead to intense and prolonged vibrations, affecting passenger comfort and potentially causing fatigue or damage to the bus body components.

For hydrogen fuel cell city buses, the actual operating conditions during daily travel are quite complex, and it is challenging to obtain and apply corresponding loads. Moreover, the vibration characteristics obtained from the free modal analysis are sufficiently close to real-world conditions. Therefore, in this study, the free modal analysis method is selected to investigate the vibration characteristics of the hydrogen fuel cell city bus.

3. Simulation Analysis of Static and Dynamic Characteristics of Bus Body Frame

3.1. Static Structural Mechanics Simulation Results

3.1.1. Horizontal Bending Condition

In Figure 3, under the horizontal bending condition, the maximum stress in the bus body frame is 220.7 MPa, and it occurs at the connection between the left side frame and the fifth beam of the roof frame. The bus body frame material adopted is Q345, with a yield strength of 345 MPa, indicating that the overall structural integrity of the bus body can meet the strength requirements for this condition.

According to Figure 4, the maximum displacement in this condition is 7.723 mm, with significant deformation concentrated mainly in the front half of the roof frame. The overall deformation of the body frame is controlled within an acceptable range of 30 mm, which does not exceed the expected target and meets the stiffness requirements for design.

3.1.2. Ultimate Torsion Condition

In Figure 5, under the ultimate torsion condition, the maximum stress in the bus body frame is 348.6 MPa, and it occurs at the welding position between the third beam of the roof frame and the second pillar of the left side frame. The bus body frame material adopted is Q345, with a yield strength of 345 MPa, and the maximum stress value exceeds the yield strength of this material, indicating that the bus body frame does not meet the strength requirements for this condition and requires redesign.

According to Figure 6, the maximum displacement in this condition is 28.401 mm, with significant deformation mainly concentrated in the right side frame area near the door. Since this condition represents the ultimate operating condition, the larger deformation is due to the right front wheel being off the ground, which aligns with the real-world situation. The overall deformation of the bus stays within the expected target, meeting the stiffness requirements for design under this condition.

3.1.3. Emergency Braking Condition

In Figure 7, under the emergency braking condition, the maximum stress in the bus body frame is 305.6 MPa, and it occurs at the connection between the lower horizontal beam under the first passenger window of the rear left side frame and the straight beam. The bus body frame material adopted is Q345, with a yield strength of 345 MPa, indicating that the overall structure of the bus body can meet the strength requirements for this condition.

Based on Figure 8, the maximum displacement in this condition is 10.045 mm, with significant deformation mainly concentrated in the middle part of the roof frame and the upper part of the rear side frame. The overall deformation does not exceed the expected target, meeting the stiffness requirements for design under this condition.

3.1.4. Emergency Cornering Condition

Based on Figure 9, under the emergency cornering condition, the maximum stress in the bus body frame is 328.9 MPa, and it occurs at the connection between the third vertical column of the right side frame and the roof frame. The material used for the bus roof frame is Q345, with a yield strength of 345 MPa. Although the maximum stress value is not exceeding the yield strength of this material, it is very close to the limit. This represents a critical condition for the bus body frame and requires a redesign.

As shown in Figure 10, the maximum displacement in this condition is 13.408 mm, with significant deformation mainly concentrated in the upper part of the right side frame and the front-middle part of the roof frame. As this condition represents a critical scenario during actual operation when the bus makes an emergency right turn, the large deformation is due to significant lateral forces acting on the bus body. The observed deformation aligns with the expected behavior. The overall deformation of the bus does not exceed the expected target, thus meeting the stiffness requirements for design under this condition.

3.2. Dynamic Modal Simulation Results

The modal analysis of the hydrogen fuel cell city bus body frame was conducted using Optistruct software 2018 (Altair, Troy, MI, USA, 2018), and the first 16 natural frequencies were extracted. Among them, the first six natural frequencies were found to be close to 0, indicating that the first six modes of the bus body frame are rigid modes, resulting in rigid displacements that are not relevant for the analysis in this study. Therefore, the first six natural frequencies were omitted from further consideration.

Table 3. Frequencies of the bus body’s first ten modes.

Order	Frequency/Hz
1	5.97
2	8.71
3	10.57
4	11.27
5	12.35
6	13.59
7	13.67
8	15.92
9	18.62
10	19.41

shows the natural frequencies for the first 10 modes of the modal analysis, with the lowest natural frequency being 5.97 Hz, which satisfies the low-frequency vibration requirements of the bus body frame.

4. Size Optimization of Bus Body Frame

4.1. Optimization Methods and Mathematical Models

Based on the static and dynamic analysis of the hydrogen fuel cell city bus body frame as mentioned above, it is evident that the maximum stress in the body frame under ultimate torsion and emergency cornering conditions is very close to or exceeds the yield strength of its material. Therefore, optimization of the bus body frame is necessary to address this issue. Since the bus body frame is constructed by welding numerous hollow rods of different thicknesses, ensuring the assembly accuracy of the body is essential. Hence, the thickness of the components is selected as the design variable for the optimization. Ultimately, this study adopts the size optimization approach to optimize the structure of the bus body frame.

In this paper, the roof beam, left and right side pillars, front and rear frames, and the chassis of the bus body frame are selected as the optimization design area, which is based on the maximum stress position and the maximum displacement position of the body frame under the condition of emergency cornering and ultimate torsion. Therefore, the components at the maximum stress and maximum displacement parts under the extreme torsion condition and the emergency cornering condition are grouped separately, and then the components with symmetrical structure and the same thickness are divided into the same group; finally, 18 groups of components are obtained. The thicknesses of these 18 groups of components are chosen as the design variables.

The objective of the optimization is to minimize the overall bus mass while ensuring that the maximum stress in the bus body frame under both ultimate torsion and emergency cornering conditions is less than the material yield strength. The optimization process involves constraining the design variables and setting upper and lower limits for the maximum stress under the two operating conditions. The ultimate goal is to achieve bus lightweighting while meeting the strength requirements of the bus body frame. The mathematical model is established as shown in the equation:

$$\{\begin{array}{ll}Find& X={[x_1,x_2,\cdots x_i]}^T\\ \min & M\\ s.t.& {\sigma }_n(X)\le 345\\ & {\sigma }_Z(X)\le 345\\ & x_i{}^L\le x_i\le x_i{}^U\\ & i=1,2,3,\cdots 18\end{array}$$

(1)

In the equation, $x_i$ represents the thickness of a component, mm; $i$ represents the number of components; ${\sigma }_n(X)$ represents the maximum stress calculated under the ultimate torsion condition, MPa; ${\sigma }_Z(X)$ represents the maximum stress calculated under the emergency cornering condition, MPa; $x_i{}^L$ and $x_i{}^U$ represent the upper and lower limits of the component thickness, in mm, respectively.

4.2. Optimization Results

After applying the size optimization method to the bus body frame and conducting 7 iterations, the final optimized results were obtained. The thickness of the optimized components was further rounded to appropriate values. The selected thickness values before and after the optimization for the components are presented in

Table 4. The thickness of rods before and after optimization (mm).

Part ID	Initial Value	Optimized Value
1	3.0	3.2
2	2.0	3.9
3	3.0	4.0
4	2.0	2.6
5	1.5	1.2
6	3.0	3.0
7	2.0	3.0
8	5.0	3.0
9	2.0	3.0
10	2.0	1.5
11	2.0	1.5
12	2.0	3.0
13	2.0	1.5
14	2.0	2.0
15	3.0	4.0
16	3.0	1.5
17	3.0	1.7
18	4.0	5.0

.

After completing the optimization process, a new finite element model of the bus body frame was reconstructed based on the rounded thickness of the optimized components. The optimized bus body frame was then subjected to static simulation tests under two target conditions, namely ultimate torsion and emergency cornering. Figure 11 illustrates the stress and displacement contour plots of the bus body frame after optimization under these two target conditions.

As shown in Figure 11a, under the ultimate torsion condition, the maximum stress value has been reduced from the original 348.6 MPa to 300.6 MPa, which is now below the yield strength of the Q345 material (345 MPa). This indicates that the optimized bus body frame can meet the strength requirements for this condition. Additionally, as depicted in Figure 11b, the maximum displacement has decreased from the original 28.401 mm to 23.658 mm, further enhancing the stiffness performance of the bus body frame under this condition.

Moving on to the emergency cornering condition, as illustrated in Figure 11c, the maximum stress value has been reduced from the original 328.9 MPa to 262.7 MPa, which is also below the yield strength of the Q345 material (345 MPa). This shows that the bus body frame has further improved its strength performance under this condition. Furthermore, as shown in Figure 11d, the maximum displacement has decreased to 12.474 mm, and it remains within the expected target, satisfying the design stiffness requirements.

Based on the results obtained from the static simulation tests under these two target conditions, the feasibility and effectiveness of the size optimization method have been demonstrated.

4.3. Validation of Simulation Results after Optimization

Due to the size optimization method, the mathematical model was only designed and optimized for two critical target conditions, namely, the ultimate torsion and emergency cornering conditions. However, it did not take into account the potential impact of changes in the body frame’s dimensions on the horizontal bending and emergency braking conditions, as well as the modal natural frequencies. Therefore, it is necessary to perform a static analysis for the optimized finite element model of the body frame under these two additional conditions, and also conduct modal analysis to validate the safety of the optimized model and the effectiveness of the optimization method.

The static simulation results of the optimized body frame under the horizontal bending and emergency braking conditions are presented in Figure 12.

As shown in Figure 12a, under the horizontal bending condition, the maximum stress value decreases to 207.3 MPa, which is lower than the yield strength of its material Q345 (345 MPa), further enhancing the strength performance of the bus body frame. Additionally, as illustrated in Figure 12b, the maximum displacement reduces to 6.116 mm, further improving the stiffness performance of the bus body frame in this condition. Moving on to Figure 12c, under the emergency braking condition, the maximum stress value decreases from 305.6 MPa to 262.4 MPa, indicating a significant improvement in the strength performance of the bus body frame after size optimization. Furthermore, Figure 12d demonstrates that the maximum displacement also decreases to 8.084 mm, enhancing the stiffness performance of the body frame during emergency braking. The static simulation analysis conducted under the other two typical conditions verifies the effectiveness of the size optimization method employed in this study in enhancing the strength and stiffness performance of the bus body frame.

4.4. Performance Comparison Analysis before and after Optimization

Based on the static simulation results of the four typical conditions conducted on the bus body frame before and after optimization, a comparison of the maximum stress and maximum displacement results is presented in

Table 5. Comparison of maximum stress and displacement for four typical operating conditions before and after optimization.

Condition	Maximum Stress (MPa)		Change	Maximum Displacement (mm)		Change
	Initial Value	Optimized Value		Initial Value	Optimized Value
Horizontal bending	220.7	207.3	−6.07%	7.723	6.116	−20.81%
Ultimate torsion	348.6	300.6	−13.77%	28.401	23.658	−16.70%
Emergency braking	305.6	262.4	−14.14%	10.045	8.084	−19.52%
Emergency cornering	328.9	262.7	−20.13%	13.408	12.474	−6.97%

.

The comparison results of the first ten natural frequencies of the bus body frame before and after optimization are shown in

Table 6. Comparison of the first ten modal frequencies before and after optimization.

Order	Initial Value (Hz)	Optimized Value (Hz)	Change (Hz)
1	5.97	6.44	0.47
2	8.71	8.82	0.11
3	10.57	10.63	0.06
4	11.27	11.32	0.05
5	12.35	12.57	0.22
6	13.59	13.65	0.06
7	13.67	14.59	0.92
8	15.92	15.97	0.05
9	18.62	18.92	0.30
10	19.41	19.68	0.27

. After optimization, the first natural frequency increases to 6.44 Hz, which is no longer within the range of external excitation resonance, meeting the design requirements of the body frame.

Under static simulation tests, according to Table 5, it can be observed that the optimization results for the selected ultimate torsion and emergency cornering, which are the two critical operating conditions in this study, are quite satisfactory. Under the ultimate torsion condition, the maximum stress in the optimized bus body frame decreased from 348.6 MPa, which exceeded the material yield strength, to 300.6 MPa, representing a reduction of 13.77% compared to the pre-optimization value, thereby meeting the design requirements for strength. Additionally, the maximum displacement decreased by 4.743 mm, accounting for a reduction of 16.70%, resulting in an improvement in the stiffness performance of the body frame. Subsequently, under the emergency cornering condition, the maximum stress was reduced to 262.7 MPa after optimization, indicating a significant reduction of 20.13% and staying far from the material’s yield strength. The maximum displacement was also reduced by 6.97% after optimization. Finally, under the other two typical operating conditions after optimization, the strength and stiffness performance of the bus body frame were improved to varying degrees. The results above validate the effectiveness of the optimization method.

In the actual operation of buses, low-frequency vibrations are often more dangerous than high-frequency vibrations. Therefore, this study focuses on analyzing the first ten mode frequencies of the bus body frame. Under the dynamic modal simulation test, a comparison of the mode frequencies before and after optimization is presented in Table 6. It is observed that after optimization, each mode frequency increases by less than 1 Hz, with the first mode frequency increasing to 6.44 Hz. Moreover, the overall modal frequencies range between 6.44 Hz and 19.68 Hz, and each mode frequency increases steadily without any significant abrupt changes. This observation indicates a well-connected and stable overall structure of the bus body frame.

During the operation of the bus, it is subjected to various types of excitations. Internal excitations mainly originate from the engine, transmission system, and electric motors, among others, while external excitations primarily come from the road surface. For the hydrogen fuel cell city bus studied in this paper, its typical operating conditions mainly involve city roads. The road surface excitations generated under urban road conditions can be calculated using the following equation [35]:

$$f=\frac{v}{3.6\times \lambda }$$

(2)

In the equation, $f$ represents the excitation frequency generated by the road surface, Hz; $v$ is the vehicle speed, km/h; and $\lambda$ is the wavelength of the road surface irregularities, m.

On urban asphalt roads, the road surface irregularity is generally taken as 7, and the chosen passenger bus has a maximum travel speed of 75 km/h. Substituting the corresponding values into the equation, the excitation frequency from the road surface is calculated to be 2.98 Hz. Since the lowest frequency of the bus body frame is 6.44 Hz, it is higher than the excitation frequency from the urban road surface, indicating that the bus will not experience resonance in the bus body while driving in the city. Furthermore, based on the relevant information provided by the company, the excitation frequency range of the internal drive shaft and the drive motor in the bus is between 30 and 40 Hz. Therefore, the vibration generated by internal excitation will also not cause resonance in the bus body frame.

Based on

Table 7. Comparison of bus body frame mass before and after optimization.

Object	Initial Value (kg)	Optimized Value (kg)	Change
mass	2107	2001	−5.03%

, it can be observed that after optimizing the passenger bus body frame, not only are the strength and stiffness requirements of the body frame design met but also the lightweighting objective is achieved. The optimized body frame exhibits a reduction in mass by 106 kg, which corresponds to a weight reduction of 5.03%. The lightweighting effect is evident, showcasing a significant improvement in the overall performance of the bus body frame.

5. Conclusions

The hydrogen fuel cell city bus has the advantages of environmental protection and long mileage, and has entered a rapid development stage in the public transportation market. In this paper, to ensure the driving safety of the hydrogen fuel cell city bus, the finite element model of the hydrogen fuel cell city bus body frame is established firstly. Then, the static and dynamic mechanical performance of the hydrogen fuel cell city bus are studied using the finite element simulation method, and the results of the static structural simulation test and dynamic modal simulation test are analyzed. The frequency of the bus body frame vibration is obtained by the dynamic modal simulation test, which allows the investigation of potential body resonance behavior. The maximum stress value and maximum displacement value are obtained by static structural simulation test, and it is found that there are two kinds of dangerous operating conditions. Based on this, the size optimization method is applied to optimize the bus body frame structure, finally achieving the driving safety of the hydrogen fuel cell city bus. The following conclusions are obtained:

(1)

The static structural simulation results indicate that the maximum stresses under horizontal bending and ultimate braking conditions are 220.7 MPa and 305.6 MPa, respectively, which meet the strength design requirements. But, in the condition of emergency cornering, the maximum stress experienced by the hydrogen fuel cell city bus body frame reaches 328.9 MPa, which approaches the material yield strength of 345 MPa. Under the condition of ultimate torsion, the maximum stress of the body frame is 348.6 MPa, exceeding the material yield strength of 345 MPa, and does not meet the strength design requirements. This suggests that the bus body frame is at risk of dangerous operation under these two driving conditions.

(2)

The results of dynamic modal simulation tests indicate that the modal frequency range of the hydrogen fuel cell city bus body frame is 5.97–19.41 Hz, which is higher than the excitation frequency of the urban road surface. Additionally, it does not fall within the frequency vibration range of the bus’s drivetrain and drive motor. Therefore, the bus body frame will not experience the resonance phenomenon.

(3)

The optimization results demonstrate that, after structural size optimization, the maximum stress of the hydrogen fuel cell city bus body frame is reduced from 328.9 MPa to 262.7 MPa in the emergency cornering condition and from 348.6 MPa to 300.6 MPa in the ultimate torsion condition; the maximum reduction is 20.13%. At the same time, the mass of the body frame is reduced by 106 kg. Furthermore, through verification, the maximum stress in the other two operating conditions is further reduced, and all these values are below the material’s yield strength of 345 MPa. Additionally, the maximum displacements in all four operating conditions are reduced to varying degrees, and the modal frequencies are appropriately increased. These findings indicate that the optimized bus body frame meets the design requirements for strength and stiffness, and it is more distant from the road surface excitation frequencies, thus ensuring the safety of the bus during operation.

Based on the above conclusions, the effectiveness of the optimization method applied to the bus body frame has been demonstrated in this paper. Moreover, while enhancing the strength and stiffness performance of the hydrogen fuel cell city bus body frame, weight reduction has been achieved, further increasing the bus’s range capability. Overall, the optimization has yielded favorable results and provides valuable insights for the company during the bus body frame design phase.