Analysis on Random Vibration and Impact Response of Vehicle-Borne Electronic Chassis

Abstract

In order to meet lightweight design requirement of vehicle-borne electronic chassis, vibration and impact response of chassis was analyzed based on the theory of random vibration and transient impact dynamics. Considering the influence of heat dissipation, corrosion resistance, material strength and economy of processing, weight reduction design was carried out according to vibration and impact response stress nephogram of chassis. The computation results show that the weight of chassis frame decreased by 16.4% and the first-order modal frequency of chassis decreased by 14.2% after weight reduction. Impact response had a lag relative to input impact spectrum. The increase of vibration stress was obviously higher than that of impact stress in different directions, which was still less than the corresponding material yield strength. That is, the structural strength of chassis after weight reduction meets the requirements of vibration and impact resistant design. The research results can provide theoretical basis of electronic equipment lightweight design under vehicle vibration and impact environment.

1 Introduction

Due to the limitation of installation space and vehicle carrying capacity, the design of vehicle-borne electronic chassis should consider miniaturization, integration and lightweight. Meanwhile, when vehicle is driving on the road, the tire collision with the ground obstacles generates non-periodic excitation load, which is transferred to chassis through car body. That is, chassis is subjected to vibration and impact load generated by vehicle transportation. Lightweight design of chassis reduces structural rigidity and strength, which is not conducive to improving its vibration and impact resistance. At present, experimental and simulation method is applied to lightweight research of electronic equipment. In recent years, based on a large number of vibration and impact test data, dynamics algorithm of finite element analysis (FEA) software is constantly improving and computation accuracy is greatly improved. Compared with experimental method, finite element method (FEM) can shorten the development cycle and reduce the cost, and is widely used in lightweight design of electronic equipment [1].

Liu [2] performed numerical calculation of random vibration response and fatigue life estimation for BGA package. Simulation results of vibration displacement response were in good agreement with experimental results, which effectively verified the reliability of FEA model. The results show that response stress increased with the increase of vibration load, and screw loosening made BGA package more likely to be damaged. Xie [3] used Adams software for kinematic simulation of RV reducer to obtain acceleration time history of spur gear. PSD function was obtained by solving autocorrelation function and Fourier transform of acceleration time history. The first six-orders modal frequencies of reducer were computed in ANSYS Workbench software, and random vibration analysis was carried out by input PSD function. According to the stress nephogram of gear, reducer had high reliability. Huang [4] established dynamic analysis model of battery pack in electric vehicle (EV) and computed its vibration response based on random vibration theory. To verify the accuracy of computation model, free modal computation data and modal test results were compared. The errors of first 4-orders modal frequencies were less than 3.3%, and modal shapes were the same, indicating that computation modal had certain reliability. According to vibration and impact experiment conditions specified in national standard of EV battery pack, steady-state random excitation load and half sine wave impact load were applied respectively. Vibration and impact stress of battery pack was less than the material strength, that is, structural strength of battery pack met the requirements of vibration and impact environment. At present, there are few researches on lightweight design of vehicle-borne electronic equipment under random vibration and transient impact.

In this paper, random vibration and transient impact of vehicle-borne electronic chassis are nalysed theoretically, and FEA model of chassis is established. Based on modal computation, random vibration spectrum and half sine wave impact spectrum are input into FEA software to nalyse vibration and impact response. Vibration and impact stress nephogramis nalysed to carry out weight reduction design. Vibration and impact response of chassis after weight reduction is computed, and the changes of stiffness and strength before and after weight reduction are compared to determine the weight reduction scheme of chassis.

2 Description of Analysis Model

Figure 1 shows the geometric model of vehicle-borne electronic chassis. The chassis consists of frame, modules, axial flow fan and switching board. The frame carries the weight of modules, axial flow fan and switching board. To meet the requirement of lightweight design, the material is aluminum alloy whose yield strength is 165 MPa. The weight of chassis is 45 kg. The weight of frame is 14.6 kg.

Fig. 1

Geometric model of vehicle-borne electronic chassis

3 Excitation Spectrum

3.1 Vibration Excitation Spectrum

The vibration excitation of chassis mainly comes from the interaction between tire and ground. Figure 2 shows the random vibration spectrum of chassis in different directions. Vibration frequencies ranged from 10 to 500 Hz. The vertical, transversal and longitudinal root mean square (RMS) of acceleration was 1.04 g, 0.204 g and 0.74 g respectively.

Fig. 2

Random vibration spectrum of chassis

3.2 Impact Excitation Spectrum

In addition to continuous random vibration load, chassis is subjected to impact load with short pulse width. The impact environment of chassis was half sine wave, peak acceleration was 15 g, pulse width was 11 ms, and impact spectrum in different directions was the same.

4 Analytical Method

4.1 Computation Method of Random Vibration

When chassis is excited by acceleration whose PSD is $P_{{\ddot{A}}} (\omega )$, the dynamic equation of random vibration is defined as [5]

$$ M\ddot{Z} + C\dot{Z} + KZ = MI\ddot{A}(t) $$

(1)

where M is the mass matrix, C the damping matrix, K the stiffness matrix, Z the displacement vector, I the acceleration vector, $\ddot{A}(t)$ the acceleration excitation.

Random vibration analysis, namely PSD analysis, is different from sinusoidal vibration which expresses dynamic equation with specific function. Probability statistics method is used to describe its stochastic process related characteristic quantities. Based on modal analysis, vibration stress, strain and deformation are computed by combining modal response statistics of each order. Input acceleration load and response data of random vibration are random variables [6, 7]. In Eqs. (1), the value of C and $\ddot{A}(t)$ is 0, and the i order modal participation factor (Q_i) is obtained by modal calculation of chassis. $Q_{i} = \beta^{T} MI$, β is the mass-normalized mode shape. According to Wiener-Khintchine theorem, response PSD ($P_{ZZ} (\omega )$) is defined as

$$ P_{ZZ} (\omega ) = \sum\limits_{i = 1}^{n} {Q_{i}^{2} \beta_{i} \beta_{i}^{T} \left| {\left. {F_{i} (\omega )} \right|} \right.^{2} P_{{\ddot{A}}} (\omega )} $$

(2)

where ω is the circular frequency, F_i(ω) the frequency transfer function.

RMS of random vibration response stress (σ_Z) is defined as

$$ \sigma_{Z} = \left[ {\int_{ - \infty }^{ + \infty } {P_{ZZ} (\omega )d\omega } } \right]^{1/2} = \left[ {\sum\limits_{i = 1}^{n} {Q_{i}^{2} \beta_{i} \beta_{i}^{T} } \int_{ - \infty }^{ + \infty } {\left| {\left. {F_{i} (\omega )} \right|} \right.^{2} P_{{\ddot{A}}} (\omega )d\omega } } \right]^{1/2} $$

(3)

4.2 Computation Method of Transient Impact

Impact response of chassis is computed by time domain analysis, whose input impact spectrum is half sine wave. Newmark iteration method in the FEA software transient structural analysis module is applied for impact computation. Newmark iteration method is defined as [8, 9].

$$ z_{k + 1} = z_{k} + \Delta t\mathop z\limits^{.}_{k} + \left( {0.5 - \eta } \right)\Delta t^{2} \mathop z\limits^{..}_{k} + \eta \Delta t^{2} \mathop z\limits^{..}_{k + 1} $$

(4)

$$ \mathop z\limits^{.}_{k + 1} = \mathop z\limits^{.}_{k} + \left( {1 - \gamma } \right)\Delta t\mathop z\limits^{..}_{k} + \gamma \Delta t\mathop z\limits^{..}_{k + 1} $$

(5)

where z is the displacement, t the time, k the iterative steps, η and γ the Newmark constant.

The principle of Newmark iteration method is to divide the impact pulse width into several uniformly distributed time substeps. Firstly, strain rate is gained by solving element node velocity of chassis model, and element strain increment is derived by integrating strain rate. Then, total element strain is acquired by summing strain of previous time step with strain increment. Finally, on the basis of the relationship between stress and strain, total element strain is transformed into stress. From the foregoing, impact stress computed by time domain analysis is close to measured stress. Impact computation has high accuracy and reliability, but is limited by the number of iterative steps, resulting in a large amount of computation.

5 Vibration and Impact Computation for Chassis

5.1 FEA Model

On the premise of not affecting the overall stiffness of chassis, the hole, fillet, boss, chamfering and other features of model were simplified. The front door, back door, roof, switching board, modules and axial flow fans were replaced by equivalent mass points [10]. Figure 3 shows the FEA model of chassis. Tetrahedral and hexahedral element was applied for meshing, whose element type was Tet10 and Hex20 respectively. The number of FEA elements was 95,511.The number of FEA nodes was 195,001 [11]. The boundary condition was defined as the inner surface of the 12 bolt holes at the bottom of chassis adopted fixed constraints.

Fig. 3

FEA model of chassis

5.2 Modal Analysis

Random vibration analysis was based on modal analysis, and modal calculation was carried out first [12]. Figure 4 shows the first six-orders mode shapes. The first 6-orders modal frequencies (Hz) were 37.518, 85.189, 145.16, 183.55, 207.06 and 247.18. It can be seen from mode shapes that the upper and lower beams had large modal deformation, whose rigidity was weak.

Fig. 4

The first six-orders mode shapes

5.3 Random Vibration Response Analysis

On the basis of modal computation of chassis, vertical, transversal and longitudinal random vibration spectrum was input respectively in the random vibration module of FEA software to compute vibration response. Random vibration spectrum was applied to the entire chassis. Figure 5a, b and c show the vertical, transversal and longitudinal random vibration 3σ stress nephogram respectively. The stress was normally distributed with a probability of 99.73% between -3σ and 3σ. Because the beams were used to support modules with large weight, vertical, transversal and longitudinal maximum stress was located in the upper beam, and maximum stress was 65.926 MPa, 25.592 MPa and 50.326 MPa respectively. Vertical stress was the largest, which was less than yield strength of beam.

Fig. 5

Random vibration 3σ stress nephogram

5.4 Transient Impact Response Analysis

Half sine wave impact spectrum in different directions was added to FEA software to compute stress. Impact spectrum was applied to the entire chassis. The number of substeps was 50. Figure 6a, b and c show the time history of vertical, transversal and longitudinal maximum stress respectively. Because impact spectrum in different directions was the same, time history of stress had the same trend, with only one peak point. Stress reached its peak at 9.86 ms, 11.11 ms and 9.33 ms, and maximum stress was 50.124 MPa, 120.59 MPa and 37.852 MPa respectively. Transversal stress was the highest. The maximum stress occurred after the peak time of input half sine wave impact, and the stress gradually decreased with the increase of time after the impact. It shows that impact response had a lag relative to input impact spectrum. Figure 7a, b and c show the vertical, transversal and longitudinal transient impact stress nephogram respectively. Similar to the results of vibration computation, maximum impact stress in three directions was located in the upper beam of chassis, which was smaller than yield strength of beam.

Fig. 6

Time history of maximum stress

Fig. 7

Transient impact stress nephogram

6 Lightweight Design of Chassis

It can be seen from Sect. 5 that the beam carried the weight of modules, resulting in high stress, which indicates that beam was not suitable for weight reduction design. The stress of sidewall, roof and floor of chassis was low, which had design space to reduce the weight. If the chassis wall was too thin in thickness, machining distortion will be greatly affected and process performance will decrease. If the weight reduction holes were designed on the side wall of chassis, the heat dissipation performance of axial flow fan will be reduced. Because the size and number of modules remained the same, weight cannot be reduced by reducing the size of chassis. Considering the influence of corrosion resistance, material strength and economy of processing, material whose density was less than aluminum alloy cannot meet the above requirements. It can be seen from the above that reducing the thickness of chassis wall was a feasible weight reduction scheme. The thickness of sidewall, roof and floor of chassis was changed from 3 to 2 mm. The weight of frame after weight reduction was 12.2 kg, which decreased by 16.4%. The weight of chassis was 42.6 kg, which decreased by 5.3% [13].

7 Vibration and Impact Computation for Chassis After Weight Reduction

7.1 FEA Model

Figure 8 shows the FEA model of chassis after weight reduction. The grid division method remained unchanged. The number of FEA elements was 82,481. The number of FEA nodes was 172,876.

Fig. 8

FEA model of chassis after weight reduction

7.2 Modal Analysis

Figure 9 shows the first six-orders mode shapes after weight reduction. The first 6-orders modal frequencies (Hz) were 32.208, 66.554, 106.45, 137.02, 176.11 and 189.46.

Fig. 9

The first six-orders mode shapes after weight reduction

Table 1 shows the first six-orders mode frequencies before and after weight reduction, f₁ is the mode frequency before weight reduction, f₂ is the mode frequency after weight reduction, p₁ is the percentage of modal frequency reduction after weight reduction. The first-order modal frequency decreased by 14.2% after weight reduction, and all modal frequencies decreased, indicating that reducing the thickness of chassis wall reduced the stiffness.

Table 1 The first six-orders mode frequencies before and after weight reduction

7.3 Random Vibration Response Analysis

Figure 10 shows the random vibration 3σ stress nephogram after weight reduction in different directions. Vertical, transversal and longitudinal maximum stress was 140.33 MPa, 57.792 MPa and 88.37 MPa respectively, which was smaller than yield strength.

Fig. 10

Random vibration 3σ stress nephogram after weight reduction

Table 2 shows the maximum vibration stress of chassis before and after weight reduction, σ₁ is the maximum vibration stress before weight reduction, σ₂ is the maximum vibration stress after weight reduction, p₂ is the percentage of stress increase after weight reduction. Vertical, transversal and longitudinal stress increased significantly after weight reduction. Transversal stress increased by 125.8%, which increased the most.

Table 2 Maximum vibration stress of chassis before and after weight reduction

7.4 Transient Impact Response Analysis

Figure 11 shows the time history of maximum stress after weight reduction in different directions. Stress reached its peak at 9.53 ms, 11.66 ms and 9.28 ms, and maximum stress was 53.075 MPa, 133.23 MPa and 39.066 MPa respectively, which was smaller than yield strength. Figure 12 shows the impact stress nephogram after weight reduction in different directions. Similar to the results of vibration computation, maximum impact stress in different directions was located in the upper beam of chassis.

Fig. 11

Time history of maximum stress after weight reduction

Fig. 12

Transient impact stress nephogram after weight reduction

Table 3 shows the maximum impact stress of chassis before and after weight reduction, σ₃ is the maximum impact stress before weight reduction, t₁ is the time when impact stress reached its peak before weight reduction, σ₄ is the maximum impact stress after weight reduction, t₂ is the time when impact stress reached its peak after weight reduction, p₃ is the percentage of stress increase after weight reduction. Vertical, transversal and longitudinal stress increased. Transversal stress increased by 10.5%, which increased the most. The increase of vibration stress was obviously higher than that of impact stress, the results show that the strength of chassis decreased after weight reduction, the change of transversal vibration and impact strength was obvious, and weight reduction had little influence on the trend of time history of maximum stress.

Table 3 Maximum impact stress of chassis before and after weight reduction

8 Conclusions

Random vibration and transient impact response of vehicle-borne electronic chassis before and after weight reduction was compared and analyzed. The weight of chassis frame decreased by 16.4%. All modal frequencies decreased, and the first-order modal frequency of chassis decreased by 14.2% after weight reduction. The maximum stress of vibration and impact was located in the upper beam. Vertical, transversal and longitudinal maximum vibration stress increased by 112.9%, 125.8% and 75.6% respectively. Impact stress reached its peak at 9.53 ms, 11.66 ms and 9.28 ms, and maximum impact stress increased by 5.9%, 10.5% and 3.2% respectively. Impact response had a lag relative to input impact spectrum. The increase of vibration stress was obviously higher than that of impact stress, which was still less than the corresponding material yield strength. The change of transversal vibration and impact strength was obvious, and weight reduction had little influence on the trend of time history of maximum stress. It indicates that the stiffness and strength of chassis after weight reduction were reduced, but it still met the requirements of vibration and impact resistant design. The design scheme for weight reduction was feasible. Lightweight design of vehicle-borne electronic equipment based on FEM can shorten the development cycle and reduce the test cost.