
==== Front
Sci Rep
Sci Rep
Scientific Reports
2045-2322
Nature Publishing Group UK London

39223226
71369
10.1038/s41598-024-71369-4
Article
Numerical study on the forward and inverse problems of the mobile pump truck frame
http://orcid.org/0000-0003-3249-5629
Zhang Yu-Liang zhang002@sina.com

1
Lin Hai-Bin 2
Zhu Zu-Chao 3
1 https://ror.org/024nfx323 grid.469579.0 College of Mechanical Engineering and Key Laboratory of Air-Driven Equipment Technology of Zhejiang Province, Quzhou University, Quzhou, 324000 China
2 grid.412246.7 0000 0004 1789 9091 College of Mechanical and Electrical Engineering, Northeast Forestry University, Harbin, 150040 China
3 https://ror.org/03893we55 grid.413273.0 0000 0001 0574 8737 The Zhejiang Provincial Key Lab of Fluid Transmission Technology, Zhejiang Sci-Tech University, Hangzhou, 310018 China
2 9 2024
2 9 2024
2024
14 2032926 2 2024
27 8 2024
© The Author(s) 2024
2024
https://creativecommons.org/licenses/by-nc-nd/4.0/ Open Access This article is licensed under a Creative Commons Attribution-NonCommercial-NoDerivatives 4.0 International License, which permits any non-commercial use, sharing, distribution and reproduction in any medium or format, as long as you give appropriate credit to the original author(s) and the source, provide a link to the Creative Commons licence, and indicate if you modified the licensed material. You do not have permission under this licence to share adapted material derived from this article or parts of it. The images or other third party material in this article are included in the article’s Creative Commons licence, unless indicated otherwise in a credit line to the material. If material is not included in the article’s Creative Commons licence and your intended use is not permitted by statutory regulation or exceeds the permitted use, you will need to obtain permission directly from the copyright holder. To view a copy of this licence, visit http://creativecommons.org/licenses/by-nc-nd/4.0/.
Aiming at the requirements of strong mobility and high flexibility of rescue and relief mobile pump trucks, this paper designs a new type of mobile pump truck frame based on existing mobile vehicle frame models. The materials used for the frame are 40Cr and Q235, and the finite element method is utilized to carry out static mechanical analysis and dynamic characteristic analysis. Simultaneously utilizing topology optimization and multi-objective genetic algorithm to optimize the design of the frame structure. The results show that the optimized pump truck frame can meet the strength design requirements of four typical working conditions: full load bending, full load torsion, emergency turning and emergency braking, while avoiding resonance phenomena caused by road surface and diesel engine vibration. Compared with the original frame model, the weight of the optimized frame is reduced by 87.88 kg, with a weight reduction rate of 10.89%, realizing the lightweight design requirements.

Keywords

Frame modification design
Finite element analysis
Topology optimization
Multi-objective optimization
Lightweight design
Subject terms

Energy science and technology
Engineering
the "Pioneer" and "Leading Goose" R&D Program of Zhejiang2022C03170 Zhang Yu-Liang issue-copyright-statement© Springer Nature Limited 2024
==== Body
pmcIntroduction

In recent years, mobile pump trucks have been widely used in the fields of flood drainage, farmland irrigation, drought relief and field water supply. However, the current emergency rescue mobile pump trucks used for rescue and relief still need to be strengthened in terms of mobility and stability, which may lead to unstable equipment operation or delayed response in emergency situations. In addition, the pump truck frame is the main load-carrying component, which needs to bear large gravity loads in the frame during operation and movement. If the strength and reliability of the frame are insufficient, it may lead to equipment damage or failure1–4. Therefore, it is necessary to develop an emergency rescue mobile pumper frame with high strength and high reliability.

Malikasab Bagawan et al. designed an electric motorcycle frame based on a bicycle frame, which was validated using torsional analysis and static simulation. Compared to traditional frames, the newly designed frame has a lighter weight and higher strength5. Deep Patel et al. provided a detailed introduction to the general design considerations and the static analysis of solar powered car frames. In order to determine the area of maximum stress, the authors used Ansys software to carry out five kinds of analysis on the roll cage: front impact, rear impact, side impact, jolt analysis and torsion analysis6. Ilham Widiyanto et al. conducted research on the materials of car frames based on finite element analysis simulation, and compared them from five aspects: stress, strain, displacement, reaction force, and safety factor. They found that steel materials are more suitable for the safety and comfort requirements of Ford GT40 sports cars7. Enrico Armamenti et al. optimized the topology of the engine mount based on its vibration behavior, thereby reducing the vibration transmitted from the engine to the frame. The results show that topology optimization effectively reduces the mass of the engine support by nearly 20%, while increasing the first natural frequency by nearly 10%, improving passenger comfort8. Javad Gholami et al. used finite element method to perform static and dynamic analysis on the excavator bracket, and optimized the design of the bracket based on the analysis results. The results showed that the weight of the bracket was reduced by 30%9. Kamarthin et al. conducted a study on the gearbox housing of E-glass tractors, and conducted static analysis on different design parameters using Ansys software. In order to assess the degree of stress and deformation in the gearbox, the study was also carried out to analyze the conventional gray cast iron gearbox and compared it with the E-Glass gearbox housing. The different combinations of various design parameters were used to provide guidance for the optimized design of the gearbox housings10.

Wei et al. proposed a universal topology design method for Wheel Angle Module (WCM) and explored the integration principles of different subsystems11. Girish Dutt Gautam et al. designed and optimized the AISI-1020 tubular steel roll cage for Formula One racing, and conducted impact tests under different conditions using Ansys software. The results indicate that AISI-1020 tubular steel is lighter and safer than traditional first order equation anti roll frames12. Sun et al. replaced the material of a torsion beam rear axle of a bus from the original steel beam to carbon fiber reinforced plastic, and then carried out the design of cross-section improvement. By studying the stiffness, maximum stress and vibration characteristics of the carbon fiber composite beam, an optimization method combining the optimization of the layup sequence and the multi-scale reliability optimization of the CFRP structure was proposed. The structural mass was reduced by 46.96% while ensuring reliability13. Mohanavel et al. investigated the torsional effect of anti-roll bar and the effect of body roll on vehicle maneuvering in a passenger car respectively, replacing the forged solid stabilizer bar with a high-strength tubular stabilizer bar, which reduces the weight of the product while improving the fuel efficiency of the vehicle. The effectiveness of the automotive anti-roll bar was determined by analyzing the structure through finite element analysis methods14. Li et al. carried out finite element analysis of the white body according to the actual working conditions of the vehicle, and calculated the bending stiffness and torsional stiffness of the body. The optimization variables were determined according to the sensitivity analysis results, and the body structure was optimized. The results show that the bending stiffness of the optimized body structure meets the stiffness requirements, while the mass of the body is reduced to meet the lightweight requirements of the optimized design15.

Behzad Vasheghani Farahani et al. used the finite element method to simulate the rollover of buses, and obtained that the internal energy released by the bus section during the loading process helps to evaluate the integrity of the bus structure, and proposed passive safety solutions if necessary16. Jay Prakash Srivastava et al. used finite element software to analyze the strength of the go-kart roll cage under different materials and pipeline thicknesses, providing reference opinions for the optimization of the go-kart roll cage in the future17. Djamaaluddin optimized the crashworthiness design of a conventional ship fender structure with variable cross-section fenders. Using finite element software to analyze eight types of mudguards, it was found that Model 4 has the best performance, but it is recommended to change the traditional mudguard design18. Ashwani Kumar et al. studied the relationship between the dynamic vibration of the transmission and the fixed constraints of the frame, evaluated the top 10 natural frequencies and corresponding vibration modes of the transmission housing using finite element analysis, and verified the results with experimental results in literature. The numerical simulation results indicate that unconstrained bolts are the cause of vibration and noise failure in the transmission case. This provides important theoretical significance for the optimization design of the transmission housing19. Hou et al. proposed a multi-objective optimization design method for the geometric shape, and laying method of carbon fiber reinforced plastic (CFRP) T-joints in automobiles. The out-of-plane bending test of CFRP composite cap nodes was carried out by the experimental method, and a finite element analysis model was established to simulate the damage process of cap nodes of cap composites. The genetic algorithm (NSGA-II) was introduced into the solution of the global optimum solution, and the radial basis function (RBF) was used to approximate the objective function, which greatly accelerated the search speed of the Pareto front20.

Current research shows that research on frame structures at home and abroad is mainly focused on conventional passenger vehicles21–24. In contrast, research on the frame structure of mobile pump trucks, which plays a crucial role in the field of emergency rescue, is still in its early stages. In a previous work, the authors used a finite element analysis method for the frame structure of an emergency rescue mobile pump truck, thus verifying the safety and reliability of the frame during operation25. This study continues to utilize the finite element method to conduct static analysis and dynamic characteristic analysis of the pump truck frame after the retrofit design. Combined with the displacement, strength and weight reduction requirements of the frame, topology optimization and multi-objective optimization design of the frame are carried out according to the analysis results, aiming to provide a scientific basis for the research and design of the future mobile pump truck frame.

Frame modification and calculation method

Frame modification design

Based on research on the load-bearing capacity, overall dimensions, and structural layout of the frame26–28, a certain wheeled excavator chassis is selected as a reference for improved design. The chassis structure of a certain wheeled excavator is shown in Fig. 1a. Remove the wheeled excavator chassis connections and other parts such as the toolbox, and remove part of the wheeled excavator chassis upper and lower cover to observe the internal structure of the chassis. The internal structure of the excavator chassis is shown in Fig. 1b. Referring to the structural characteristics of a wheeled excavator chassis, and combined with the design principles and functional requirements of the emergency rescue mobile pump truck. This paper decides to use the combination of longitudinal beams and cross beams welding to build the frame skeleton. The two longitudinal beams and two cross beams are fixed to each other using the form of welding, and the frame skeleton model is shown in Fig. 1c. Comprehensive consideration of the diesel engine, self-priming pump, batteries and other on-board equipment, and finally get the modified original frame model, the original frame model is shown in Fig. 1d, the frame modification design process is shown in Fig. 1. In addition, in order to meet the structural and load-bearing requirements, the cross-section forms of the longitudinal and cross beams are selected to be square, with the longitudinal beam section having a height of 160 mm, a width of 110 mm, and a wall thickness of 10 mm. The cross beams are also cut from square section steel pipes, and the cross-sectional dimensions of the cross beam are consistent with those of the longitudinal beam.Fig. 1 Design process of frame modification.

Computation model

The frame model of the emergency rescue mobile pump truck has a length of 3342 mm, a width of 1700 mm, and a height of 734 mm. When using ANSYS WORKBENCH 19.2 for finite element simulation of the frame in this article, the more accurate the 3D model of the frame is constructed, the higher the reliability of the simulation results. The material parameter settings must be real, and the results of the analysis will be closer to the actual. At the same time, taking into account the complexity of the frame structure, there are some subtle geometric features. Therefore, the frame model needs to be simplified moderately to improve the analysis efficiency. By dealing with the process holes in the frame structure, smaller chamfers, smaller fillets and other interference factors to simplify the processing, so that it does not affect the overall analysis results while improving the accuracy of the calculation. The simplified frame model is shown in Fig. 2.Fig. 2 Simplified frame model.

In order to improve the simulation speed, various components of the frame load are applied to the frame based on their weight in the form of uniform loads, such as high flow self-priming pump, diesel engine, battery pack, fuel tank and cooling water tank. The main components and their weights are shown in Table 1. The material parameters of each part of the frame are shown in Table 2.Table 1 List of frame load (kg).

Name	Weight	
Self-priming pump	600	
Diesel engine	600	
Cooling water tank	400	
Battery pack	70	
Fuel tank (including fuel)	200	

Table 2 Frame material parameters.

Name	Material	Density (g cm−3)	Poisson’s ratio	Elastic modulus (GPa)	Yield strength (MPa)	
Axles, axle brackets, steering devices	40Cr	7.85	0.3	211	785	
Longitudinal beam, cross beam, other components	Q235	7.85	0.3	210	235	

The fourth strength theory is used to verify the strength of the frame. When the stress at a certain point in the frame model exceeds the material yield strength limit, plastic deformation will occur. The equivalent stress calculation formula is:1 σr=12σ1-σ22+σ2-σ32+σ3-σ12

2 σr≤σ

The [σ] in the above equation is the allowable stress. When the equivalent stress of the frame obtained from the calculation is greater than the allowable stress, the frame may be damaged.

Grid independent verification

This study applies loads to various parts of the frame and applies fixed constraints at wheel positions. During the solution process, this study gradually refined the grids while ensuring the constraints and loads remain unchanged29, and performed finite element analysis on the frame model with different numbers of grid divisions. The calculation results are shown in Fig. 3. From the figure, it can be seen that when the number of grids increases from 157,171 to 5,166,565, the maximum stress changes sharply, indicating that the number of grids has a significant impact on the calculation results. However, when the number of grids reached 6,432,829, the maximum stress remained almost unchanged after further increasing the number of grids. Therefore, for the static analysis of the frame, the number of grids is kept between 6.4 and 6.6 million in this study.Fig. 3 Maximum stress of the frame changes with the number of grids.

Boundary conditions

This study uses finite element analysis method to conduct numerical calculations under four operating conditions: full load bending, full load torsion, emergency turning and emergency braking of the vehicle frame. The loads of each component carried by the frame are applied to the corresponding positions as shown in Table 1 above, and the boundary conditions of each working condition of the frame are set up as shown in Table 3 (transverse: X, vertical: Y, longitudinal: Z, U is the translational degree of freedom, ROT is the rotational degree of freedom, and the rest of the working conditions are the same).Table 3 Boundary condition settings for each operating condition.

Working condition	Left-front wheel	Right-front wheel	Left-rear wheel	Right-rear wheel	
Full load bending	UX, UY, UZ	UX, UZ	UY, UZ	UZ	
Full load torsion	None	UX, UY, UZ	All	All	
Emergency turning	UX, UY, UZ	UY, UZ	UX, UY	UY	
emergency braking	UX, UY, UZ	UY, UZ	UX, UY	UY	

In order to more accurately obtain the stress situation of the main load-bearing components on the frame, the longitudinal beams and axles of the frame are monitored in this study for displacements and stresses. Considering that the axles and longitudinal beams of the frame are hollow structures, monitoring paths are added to the upper surface of these four critical components (1: start point, 2: end point). Among them, the monitoring path of the upper surface of the longitudinal beam is added at the centerline of the surface, and the monitoring path of the upper surface of the axle is added at the edge line near the middle of the frame, and the schematic diagram of the monitoring path is shown in Fig. 4.Fig. 4 Schematic diagram of the monitoring path.

Mechanical analysis

Static analysis

Full load bending condition

The displacement calculation results for the full load bending condition of the frame are shown in Fig. 5. The maximum displacement of the frame occurs at the battery mounting location, with a maximum displacement of 1.29 mm. The frame displacement gradually becomes larger from both ends to the middle, and the displacement at the middle of the left longitudinal beam is larger than that at the middle of the right longitudinal beam, but both are less than 1 mm. The main reason for this deformation is that the longitudinal beam bears the gravity load of the diesel engine and self-priming pump, and the diesel fuel tank installed on the left side of the frame has a larger weight.Fig. 5 Displacement distribution of the frame under bending conditions.

From Fig. 6a, taking the right end of the front and rear axles (A-1 and B-1) as the starting point, the displacement of the front axle gradually increases from 0.26 mm to the maximum displacement of 0.42 mm in the middle (at 51.2% of the axle), and then gradually decreases to 0.27 mm as the distance increases. The displacement trends of the front and rear axles are approximately the same, but the overall displacement of the rear axle is less than that of the front axle. Compared to the front axle, the minimum displacement of the rear axle is 0.18 mm, and its maximum displacement is 0.36 mm, with the maximum displacement occurring at 52.7% of the axle position.Fig. 6 Displacement curve of main components under full load bending condition. (a) Axle displacement. (b) Longitudinal beam displacement.

From Fig. 6b, it can be seen that the displacement trends of the left and right longitudinal beams are consistent, starting from the front end of the longitudinal beam (C-1 and D-1). The displacement of the longitudinal beam shows a phenomenon of first increasing and then decreasing from the front to the end, with the maximum displacement occurring at 48.8% of the longitudinal beam. For the left longitudinal beam, the displacement at the front end is 0.19 mm, the maximum displacement in the middle is 0.75 mm, and the displacement at the end is 0.04 mm. For the right longitudinal beam, the displacement at the front end is 0.20 mm, the maximum displacement in the middle is 0.70 mm, and the displacement at the end is 0.039 mm. Under the full load bending condition, the overall displacement of the frame and the displacement of each key components are small.

From Fig. 7, it can be seen that the maximum stress of the frame under full load bending condition occurs on the bracket, which is located at the connection between the front axle and the base of the right longitudinal beam, and the maximum stress is 126.02 MPa. The yield strength of the material used at the maximum stress of the frame is 785 MPa, the safety coefficient is 1.5, and the permissible stress is 523 MPa, the frame meets the design requirements and there is a certain design margin.Fig. 7 Stress distribution of the frame under full load bending condition. (a) Overall distribution. (b) local amplification.

From Fig. 8a, the stress on the front and rear axles shows a trend of first increasing and then decreasing from both ends to the middle, and rapidly increases when approaching the outer axle bracket. The peak stresses of the front axle occurred at 15.9% and 84.1% of the axle positions, with peak stresses of 112.56 MPa and 102.09 MPa respectively. The peak stresses of the rear axle occurred at 23.4% and 76.6% of the axle positions, with peak stresses of 52.90 MPa and 64.0 MPa respectively. The maximum stress on both sides of the front and rear axles does not exhibit symmetry, which may be caused by the asymmetric load borne by the frame. Due to the front wheel steering components, the length of the front axle is shorter than that of the rear axle, so the position of the front and rear axle brackets in the axle ratio is different when converting the axle ratio. In addition, the action of the inner and outer axle brackets causes two stress fluctuations during the stress drop from the outer axle bracket to the middle position of the axle.Fig. 8 Stress curve of main components under full load bending condition. (a) Axle stresses. (b) Longitudinal beam stresses.

Figure 8b represents the stress trend in the midline of the upper surface of the longitudinal beam. From the front end of the longitudinal beam to 18.4% of the longitudinal beam position, the stress of the longitudinal beam fluctuates between 1.21 and 3.56 MPa. In the two intervals of 18.4–23.9% and 40.3–46.3% of the longitudinal beam position, the stresses of longitudinal beam showed a significant decrease and then rebound phenomenon. This is mainly because the cooling water tank and diesel engine are both fixed on the longitudinal beam through the connector, which makes the stress at the contact area between the longitudinal beam and the bottom of the connector reduced, and the stress value at the front and rear end faces of the connector in contact with the longitudinal beam is larger; 66.7% to 79.6% of the longitudinal beam positions are the connecting parts for installing the self-priming pump, and the overall stress shows a decreasing trend. However, at its front and rear end surfaces in contact with the longitudinal beam, there is a smaller magnitude of wave peaks in the stresses, which is consistent with the actual situation under full load bending conditions.

Full load torsion condition

The displacement calculation results of the frame under full load torsion condition are shown in Fig. 9. When the left-front wheel is suspended, the constraint asymmetry causes more gravity load on the left-front area of the frame. The maximum displacement of the frame occurs at the position of the left-front wheel, and the trend of displacement gradually decreases from the left-front wheel to the right-rear wheel, with a maximum displacement of 10.11 mm.Fig. 9 Displacement distribution of the frame under full load torsion condition.

From Fig. 10a, due to the suspension of the left-front wheel, the displacement of the front axle continuously increases from 1.93 mm at the right end of the axle (A-1) to 8.07 mm at the left end; Compared to the front axle, the displacement trend of the rear axle fluctuates less. The maximum displacement of the rear axle occurs at 70.6% of the axle position, and the displacement at both ends of the axle are less than 0.01 mm.Fig. 10 Displacement curve of main components under full load torsion condition. (a) Axle displacement. (b) Longitudinal beam displacement.

From Fig. 10b, taking the front end of the longitudinal beams (C-1 and D-1) as the starting point, the displacement changing trends of the left and right longitudinal beams remain the same. The displacement change of the longitudinal beam shows a phenomenon of first decreasing and then increasing from the front to the end, and the displacement change of the left longitudinal beam is greater than that of the right longitudinal beam. The displacement of the left longitudinal beam continuously decreases from 8.31 mm at the front to 0.56 mm, and then increases to 1.35 mm at the end; the displacement of the right longitudinal beam continuously decreases from 4.47 mm at the front to 0.53 mm, and then increases to 1.08 mm at the end. This phenomenon occurs because when the support state of the left-front wheel changes, the main support point of the longitudinal beam shifts to the rear axle, causing slight displacement at the end of the longitudinal beam.

Based on Figs. 9 and 10, it can be seen that the maximum displacement of the frame occurs in the left half under torsional conditions, with a maximum displacement of 10.11 mm, while the displacement of the right half of the frame is less than 4.50 mm. The displacement on the left side of the frame is greater than the displacement on the right side, which shows that the full load torsional conditions is a the most dangerous working condition during vehicle driving. Therefore, such conditions should be avoided as much as possible during driving.

From Fig. 11, it can be seen that the maximum stress on the frame occurs on the axle bracket at the connection between the front axle and the base of right longitudinal beam, with a maximum stress of 294.49 MPa. This is caused by the suspension of the left-front wheel, which leads to asymmetric support of the frame. When the safety factor takes 1.5, the allowable stress of the front support plate is 523.33 MPa, which is much larger than the maximum stress of the frame. It can be seen that the strength of the frame meets the design requirements and there is a certain design margin.Fig. 11 Stress distribution of the frame under full load torsion condition. (a) Overall distribution. (b) Local amplification.

From Fig. 12a, the stress variation trend of the front and rear axles is exactly opposite. Starting from the right end of the axle (A-1 and B-1), the overall stress on the front axle shows a trend of increasing first and then decreasing. The stress increases rapidly when approaching the outer axle bracket, meaning that the maximum stress on the front axle occurs at 15.9% of the axle position, with a maximum stress of 262.56 MPa; when the stress curve crosses the highest point, the stress rapidly decreases from 262.56 to 34.31 MPa at 17.4% of the axle position, and then slowly decreases. At the position of 74.6% to 84.1% of the axle, there is a slight fluctuation in the stress curve, and the peak stress occurs at the end face of the left axle bracket.Fig. 12 Stress curve of main components under full load torsion condition. (a) Axle stress. (b) Longitudinal beam stress.

From Fig. 12b, it can be seen that the stress variation of the longitudinal beam fluctuates more significantly. At the connection between the longitudinal beam and other components, the stresses appear to decrease significantly and then rebound, and the change trends of the left and right longitudinal beams are roughly equal. Due to the asymmetric support of the frame, there are differences in the peak stresses between the left and right longitudinal beams, and the maximum stress value of the left longitudinal beam is higher than that of the right longitudinal beam. The maximum stress at various parts of the frame is much smaller than the allowable stress of its material, so the strength of the frame meets the design requirements under torsional conditions.

Emergency turning conditions

The displacement calculation results of the mobile pump truck frame under emergency turning conditions are shown in Fig. 13. The maximum displacement under this working condition occurs at the installation position of the battery, with a maximum displacement of 1.30 mm. From the overall perspective of the frame, the displacement change of the frame gradually increases from both ends to the middle when turning left, and the maximum displacement occurs in the middle of the left longitudinal beam of the frame, with a maximum displacement of 0.75 mm in the middle of the frame.Fig. 13 Displacement distribution of frame under emergency turning conditions.

From Fig. 14a, the displacement of the front axle gradually increases from 0.26 mm at the starting point (A-1) at the right end to reach the maximum displacement of 0.42 mm at the middle 50.7% axle position, after which it decreases with increasing distance. The displacement trends of the front and rear axles remained consistent. Compared to the front axle, the displacement of both ends of the rear axle is 0.19 mm, and the maximum displacement of the center is 0.36 mm.Fig. 14 Displacement curve of main components under emergency turning condition. (a) Axle displacement. (b) Longitudinal beam displacement.

From Fig. 14b, it can be seen that the displacement trends of the left and right longitudinal beams are consistent, and the displacement changes of the longitudinal beams from the front to the end show the phenomenon of increasing first and then decreasing. The displacement of the left longitudinal beam increases from 0.19 mm at the front to 0.74 mm at 48.8% of the longitudinal beam position, and then decreases to 0.04 mm at the end; the displacement of the right longitudinal beam increases from 0.20 mm at the front to 0.71 mm at 48.8% of the longitudinal beam position. The overall displacement of the frame and the displacement of each key component under emergency turning conditions are small.

From Fig. 15, it can be seen that the maximum stress of the frame under emergency turning condition also occurs in the bracket at the connection between the front axle and the base of the right longitudinal beam, and the maximum stress is 129.85 MPa. The permissible stress of the axle bracket is 523.33 MPa, which is greater than that of the frame under turning condition, and the strength of the frame meets the design requirements.Fig. 15 Stress distribution of frame under emergency turning condition. (a) Overall distribution. (b) Local amplification.

As shown in Fig. 16a, the stress curves on the monitoring paths of the front and rear axles under the emergency turning condition are shown, and the trend of stress change is approximately the same as that of the full load bending condition. The stresses on the front and rear axles first increase and then decrease from the ends of the axles to the center, and the stresses increase rapidly when approaching the outer axle bracket. The maximum stresses of the front axle are located at 15.9% and 84.1% of the axle positions, with the maximum stresses of 115.98 MPa and 98.60 MPa respectively; the maximum stresses of the rear axle are located at 23.4% and 76.6% of the axle positions, with the maximum stresses of 54.4 MPa and 61.48 MPa respectively. During the stress curve change, the stress at the contact end face of the axle with the bracket will show a large change, such as at 24.9% and 75.1% of the axle position of the front axle and 23.4% and 76.6% of the axle position of the rear axle.Fig. 16 Stress curve of main components under emergency turning condition. (a) Axle stresses. (b) Longitudinal beam stresses.

From Fig. 16b, it can be seen that from the front of the longitudinal beam to the 18.4% position of longitudinal beam, the longitudinal beam stress fluctuates within the range of 1.21–3.50 MPa. At the front and rear end faces of diesel engine installation connectors, namely in the 18.4–23.9% of the longitudinal beam position and 40.3–46.3% of the longitudinal beam position, the longitudinal beam stress shows a significant decrease and then increases; 66.7–79.6% of the longitudinal beam positions are the installation connection positions of the self-priming pump, and the overall stress shows a decreasing trend. However, there are small peaks of stress at the contact points between the front and rear end faces and the longitudinal beam.

Emergency braking conditions

The displacement calculation results of the mobile pump truck frame under emergency braking conditions are shown in Fig. 17. The maximum displacement under emergency braking conditions also occurs at the installation position of the battery, with a maximum displacement of 1.26 mm. From the overall perspective of the frame, the displacement of the frame gradually increases from both ends to the middle, and the maximum displacement occurs in the middle of the left longitudinal beam of the frame. The maximum displacement of the middle section of the frame is 0.72 mm.Fig. 17 Displacement distribution of frame under emergency braking conditions.

From Fig. 18a, starting from the right end of the front and rear axles (A-1 and B-1), the displacement of the front axle gradually increases from 0.28 mm to the maximum displacement of 0.45 mm in the middle, and then gradually decreases to 0.29 mm as the distance increases. The displacement trend of the rear axle remains consistent with that of the front axle, but the overall displacement of the rear axle is smaller than that of the front axle. Compared to the front axle, the minimum displacement of the rear axle is 0.12 mm and the maximum displacement is 0.32 mm.Fig. 18 Displacement curve of main components under emergency braking conditions. (a) Axle displacement. (b) Longitudinal beam displacement.

From Fig. 18b, taking the front end of the longitudinal beam (C-1 and D-1) as the starting point, the displacement trends of the left and right longitudinal beams remain consistent, and the displacement changes from the front end of the longitudinal beam to the rear end of the longitudinal beam show a phenomenon of first increasing and then decreasing in the direction of the longitudinal beam, with the maximum displacement occurring at the 49.8% position of the longitudinal beam. Among them, the displacement of the front end of the left longitudinal beam is 0.21 mm, the maximum displacement in the middle is 0.72 mm, and the displacement of the rear end of the longitudinal beam is 0.16 mm. The displacement of the front end of the right longitudinal beam is 0.22 mm, the maximum displacement in the middle is 0.67 mm, and the displacement of the rear end is 0.16 mm. Under emergency braking conditions, the overall displacement of the frame and the displacement of various key components are relatively small.

From Fig. 19, it can be seen that the maximum stress position of the frame under emergency braking conditions occurs on the bracket at the connection between the front axle and the base of right longitudinal beam, with a maximum stress of 177.2 MPa. The maximum stresses generated here are due to the combined effect of the diesel engine and the self-priming pump in the gravity and longitudinal inertia forces, resulting in greater loads on the front wheel bearings, causing the maximum stresses to be generated at the longitudinal beam support bracket and front wheel axle connection.Fig. 19 Stress distribution of the frame under emergency braking conditions. (a) Overall distribution. (b) Local amplification.

From Fig. 20a, the stresses of the front and rear axles change from the both ends of the axles to the middle in a trend of first increasing and then decreasing, and the stresses increase rapidly when approaching the outer axle bracket. The two larger stress peaks of the front axle occurred at 15.9% axle position and 84.1% axle position, with peak stresses of 158.39 MPa and 139.38 MPa, respectively; the stress peaks of the rear axle occurred at 23.4% axle position and 76.6% axle position, with maximum stresses of 55.86 MPa and 67.04 MPa respectively.Fig. 20 Stress curve of main components under emergency braking conditions. (a) Axle stress. (b) Longitudinal beam stress.

Figure 20b shows the trend of stress variation at the midline of the upper surface of the longitudinal beams. From the front end of the longitudinal beam to the 18.4% longitudinal beam position, the longitudinal beam stress fluctuates between 1.22 MPa and 3.93 MPa. In the two ranges of 18.4% to 23.9% longitudinal beam position and 40.3–46.3% longitudinal beam position, the longitudinal beam stress shows a significant decrease and then rebounds. This is mainly because the heat dissipation tank and diesel engine are fixed to the longitudinal beam through connectors, which reduces the stress at the contact area between the longitudinal beam and the bottom of the connector. The stress value at the contact area between the front and rear end faces of the connector and the longitudinal beam is relatively large; 66.7% to 79.6% of the longitudinal beam positions are the installation connection positions of the self-priming pump, and the overall stress shows a decreasing trend. However, there are small peaks of stress at the contact points between the front and rear end faces and the longitudinal beam.

Modal analysis

When the excitation frequency approaches the natural frequency of the frame, resonance occurs in the frame30. In order to avoid the occurrence of frame resonance, modal analysis needs to be conducted in the early design stage. This study used Ansys Workbench software to conduct finite element modal analysis on the frame, with the same constraint conditions as the full load bending condition. The first eight vibration modes and natural frequencies of the frame were calculated. The constraints of modal analysis are shown in Table 4.Table 4 Constraints for modal analysis.

Constraint position	Left-front wheel	Right-front wheel	Left-rear wheel	Right-rear wheel	
Constrained degrees of freedom	UXUYUZ	UXUZ	UYUZ	UZ	

The modal analysis of the frame reveals that the restrained intrinsic frequencies of the frame for the first eight orders range from 22.031 to 67.627 Hz. The first eight orders of intrinsic frequency and vibration mode characteristics of the frame are shown in Table 5.Table 5 First eight orders of intrinsic frequency and Vibration mode characteristics of the frame.

Order	Intrinsic frequency (Hz)	Vibration mode characteristics	Maximum deformation (mm)	
1	22.031	Overall positive bending along the x-direction	1.32	
2	30.453	Hanger fixture bent around x-axis	6.60	
3	31.646	Hanger fixture bent around x-axis	6.81	
4	40.67	Overall bending around the y-axis, the axle bending around the x-axis	2.02	
5	52.049	Torsion around the x-axis as a whole	3.39	
6	55.016	Torsion of suspension fixture around y-axis	4.39	
7	59.412	The suspension fixture is bent around the y-axis, and the rear axle is bent around the x-axis	4.03	
8	67.627	The suspension fixture is twisted around the y-axis, and the rear axle is bent around the z-axis	3.77	

The purpose of modal analysis is to determine the frequencies of each order, ensuring that the intrinsic frequency of the frame avoids the excitation frequency of external loads. The sources of frame resonance include external excitation and internal power sources, such as road excitation and engine vibration excitation. According to relevant literature31,32, road excitation is usually less than 20 Hz, and the first order vibration frequency of the vehicle body must be above 20 Hz, preferably within 25 Hz. The first-order intrinsic frequency of this frame structure is 22.031 Hz, which can avoid resonance caused by the road.

In addition, the excitation frequency of diesel engines can be obtained from Eq. (3):3 f=2nz60τ

where n—engine speed, r/min; z—number of engine cylinders; τ—number of engine strokes.

In this design, the mobile pump truck adopts a six cylinder and four stroke diesel internal combustion engine with a rated speed of 1500 r/min. The calculation show that the diesel engine vibrates at a frequency of 75 Hz when the mobile pump truck is performing normal dewatering operations. The first eight intrinsic frequencies of the full load bending condition of the frame are lower than the vibration frequency of the diesel engine, so the emergency rescue mobile pump truck will not experience resonance during normal operation.

Harmonic response analysis

This study uses Ansys Workbench software to couple the Model and Harmonic Response modules, and conducts harmonic response analysis on the frame model. A force of 500 N in the z-direction is applied as input excitation at each of the four-wheel positions. According to the results of modal analysis above, the input frequency excitation range of frequency response analysis is set to 0–70 Hz, and the modal damping coefficient is 0.05. Based on the results of static and modal analyses, the nodes in the stress-sensitive and displacement-sensitive areas of the frame are extracted for frequency response analysis in this study. The selected nodes and corresponding positions are: the frame bracket at the connection between the front axle and the base of right longitudinal beam (point A), the frame bracket at the connection between the rear axle and the base of left longitudinal beam (point B), the connection between the front of the diesel engine and the left longitudinal beam (point C), the connection between the rear of the diesel engine and the left longitudinal beam (point D), the midpoint position of the left longitudinal beam (point E), and the connection between the self-priming pump and the left longitudinal beam (point F). The corresponding positions of each response node are shown in Fig. 21.Fig. 21 Corresponding positions of response nodes.

Extract the frequency response analysis results and obtain the displacement response curves and stress response curves of the response nodes in the three directions of XYZ, as shown in Figs. 22 and 23. The peak values and corresponding frequencies of the response curves for each node are listed in Table 6.Fig. 22 Response curve of node displacement frequency.

Fig. 23 Response curve of node stress frequency.

Table 6 Calculated weights of four typical working conditions.

Working condition	Full load bending	Full load torsion	Emergency braking	Emergency turning	
Weight value	0.5485	0.2966	0.1018	0.0531	

Combined with Figs. 22 and 23, it can be seen that the wave peaks of the frame displacement and stress response curves appear near the frequencies of 22 Hz, 40.5 Hz and 59 Hz. The peaks of the frequency response correspond to the intrinsic frequency of the whole vehicle model, which verifies the reasonableness of the results of the modal frequency response analysis of the whole vehicle. However, the displacement and stress values generated by the frame at frequencies of 22 Hz, 40.5 Hz, and 59 Hz are very small, and the frequency of the diesel engine is 75 Hz. When the diesel engine operates smoothly, the frame of the mobile pump truck will not resonate.

Topological optimization

In this study, the Topology Optimization module of Ansys Workbench is used to optimize the topology of the emergency rescue mobile pumper frame for multiple working conditions33,34, and the boundary conditions of each working condition are taken as the constraints, and the minimum flexibility of the frame is taken as the objective function, so that the topology optimization of the emergency rescue mobile pumper frame model is designed by using the variable density method. Set the optimized volume fraction to 30% and the penalty factor to 3. And the weight values of four typical operating conditions are determined using the Analytic Hierarchy Process, and the calculated weight ratios of the four typical operating conditions were brought into the topology optimization mathematical model. The calculated weight values of the four typical operating conditions are shown in Table 6

Result analysis

According to the topology optimization results, there is significant optimization space at the front and rear ends of the longitudinal beam, as well as at the small and large beams in front and rear. The topology optimization results of the emergency rescue mobile pump truck frame under multiple working conditions are shown in Fig. 24.Fig. 24 Topology optimization results for multiple operating conditions.

According to the results of topology optimization, there is a significant margin for the longitudinal, small, and large beams of the frame, which can be redesigned to reduce the use of materials and reduce the weight of the frame. The longitudinal beams and small cross beams are still rectangular and partially hollowed out, while the large cross beam cross-section shape is changed from the original rectangular design to a groove design. A comparison of the frame components before and after optimization is shown in Fig. 25, and the frame model after topology optimization is shown in Fig. 26.Fig. 25 Comparison of frame components before and after optimization. (a) Front part of longitudinal beam; (b) rear part of longitudinal beam; (c) small cross beam; (d) large cross beam.

Fig. 26 Frame model after topology optimization.

Performance comparison

In order to verify the performance of the optimized frame, the static analysis and modal analysis of the frame are carried out. The results of the static calculation of the optimized frame under full load bending condition are shown in Fig. 27. It can be seen that the maximum displacement of the optimized frame under full load bending condition also occurs at the battery installation position, and the maximum displacement is 1.32 mm, which is 2.33% larger than that before optimization. The maximum stress location of the frame also occurs in the frame bracket at the connection between the front axle and the base of the right longitudinal beam, and the maximum stress is 121.88 MPa, which is 3.29% less than that before optimization.Fig. 27 Calculation results of full load bending condition after optimization. (a) Displacement distribution. (b) Stress distribution.

The static calculation results of the optimized frame under full load torsion condition are shown in Fig. 28. The maximum displacement of the optimized frame under this working condition occurs at the position of the left-front wheel, the maximum displacement is 11.47 mm, which is 1.36 mm larger than that before optimization. The maximum stress position of the frame has changed, and the maximum stress occurs on the axle bracket at the connection between the rear axle and the base of left longitudinal beam. The maximum stress is 295.17 MPa, which is 0.68 MPa higher than before optimization.Fig. 28 Calculation results of full load torsion condition after optimization. (a) Displacement distribution. (b) Stress distribution.

The static calculation results of the frame after topology optimization under emergency turning conditions are shown in Fig. 29. The maximum displacement of the optimized frame under this working condition occurs at the installation position of the battery, with a maximum displacement of 1.34 mm, which is 3.07% larger than that before optimization. The maximum stress location of the frame occurs on the bracket at the connection between the front axle and the base of the right longitudinal beam, and the maximum stress is 126.53 MPa, which is reduced by 2.56% compared with the pre-optimization.Fig. 29 Calculation results of emergency turning conditions after optimization. (a) Displacement distribution. (b) Stress distribution.

The static calculation results of the frame after topology optimization under emergency braking conditions are shown in Fig. 30. The maximum displacement of the optimized frame under this working condition also occurs at the installation position of the battery, with a maximum displacement of 1.30 mm, which is 3.17% larger than that before optimization. The maximum stress position of the frame occurs on the frame bracket at the connection between the front axle and the base of the right longitudinal beam, and the maximum stress is 167.11 MPa, which is 5.69% less than that before optimization.Fig. 30 Calculation results of emergency braking conditions after optimization. (a) Displacement distribution. (b) Stress distribution.

In order to verify the dynamic characteristics of the frame after topology optimization, the first eight modal frequencies of the frame are calculated and analyzed, and the modal shape diagram is shown in Fig. 31. The first eight steps of the optimized pump truck frame have no significant changes compared with the intrinsic frequency value of the original frame, and can avoid the excitation frequency caused by the road surface and engine. The results indicate that the optimized frame can avoid resonance and its dynamic characteristics meet safety conditions.Fig. 31 The first eight vibration modes of the frame. (a) First-order vibration mode. (b) Second-order vibration mode. (c) Third-order vibration mode. (d) Fourth-order vibration mode. (e) Fifth-order vibration mode. (f) Sixth -order vibration mode. (g) Seventh-order vibration mode. (h) Eighth-order vibration mode.

The performance comparison of the pump truck frame before and after topology optimization is shown in Table 7. The weight of the frame after topology optimization is 730.51 kg, which is reduced by 76.75 kg (9.5%) compared with the original frame. The overall performance of the topology optimized frame meets the safety requirements and the structure design is reasonable.Table 7 Performance comparison of the frame before and after topology optimization.

Variable	Original	Optimized	Variation	
Weight (kg)	807.26	730.51	− 76.75	
Full load bending condition	ω (mm)	1.29	1.32	 + 0.03	
σ (MPa)	126.02	121.88	− 4.14	
Full load torsion condition	ω (mm)	10.11	11.47	 + 1.36	
σ (MPa)	294.49	295.17	 + 0.68	
Emergency turning conditions	ω (mm)	1.30	1.34	 + 0.04	
σ (MPa)	129.85	126.53	− 3.32	
Emergency braking conditions	ω (mm)	1.26	1.30	 + 0.04	
σ (MPa)	177.2	167.11	− 10.09	
Intrinsic frequency (Hz)	First-order	22.031	22.608	 + 0.577	
Second-order	30.453	28.471	− 1.982	
Third-order	31.646	29.939	− 1.707	
Fourth-order	40.67	41.154	0.484	
Fifth-order	52.049	46.138	− 5.911	
Sixth-order	55.016	47.138	− 7.878	
Seventh-order	59.412	50.246	− 9.166	
Eighth-order	67.627	65.442	− 2.185	

Optimization design based on response surface methodology

Objective function and constraints

The topology optimization results indicate that the maximum stress and maximum displacement of the optimized frame structure still meet the strength requirements under four typical working conditions, indicating the possibility of further lightweight. In order to reduce computational complexity, this study selects the maximum stress of the frame under full load bending and full load torsion conditions as the calculation conditions. Setting the maximization of the first-order intrinsic frequency of the frame, the minimization of the weight, the minimization of the peak stress in the full-load bending condition and the full-load torsion condition as the optimization objectives, the mathematical model for the multi-condition multi-objective optimization of the frame is shown in Eq. (4).4 max:fxmin:Mx,σ1x,σ2xximin<xi<ximax

where x—the set of design variables; f(x)—first-order intrinsic frequency of the frame, Hz; σ1(x)—maximum stress of the frame under full load bending condition, MPa; σ2(x)—maximum stress of the frame under full load torsion condition, MPa; M(x)—weight of the frame, kg; ximin and ximax—upper and lower limits of each design variable.

Selecting design variables

Considering the convenience of installation, set the height of the longitudinal beams and cross beams to be the same. Therefore, when designing the lightweight frame, five factors are selected as the design variables, which are the height, thickness and width of the longitudinal beam section and the thickness and width of the cross beam section. And set the initial values and ranges of each factor, and the relevant parameters are shown in Table 8.Table 8 Initial values and ranges of design variables.

Design variable	Symbol	Initial value	Range	
Longitudinal beam height	X1	160	[140, 180]	
Longitudinal beam thickness	X2	8	[6, 10]	
Longitudinal beam width	X3	110	[90, 130]	
Cross beam thickness	X4	8	[6, 10]	
Cross beam width	X5	110	[90, 130]	

Experimental design

Box–Behnken method is selected for experimental design and 41 groups of experimental samples are taken according to the values range of design variables in Table 8. According to each group of sample points re-modeling for calculation, the Box-Behnken sample points and responses obtained are shown in Table 9.Table 9 The Box-Behnken sample points and responses.

Order	X1 (mm)	X2 (mm)	X3 (mm)	X4 (mm)	X5 (mm)	f (Hz)	M (kg)	P1 (MPa)	P2 (MPa)	
1	160	8	110	8	110	22.608	730.51	121.88	295.17	
2	140	6	110	8	110	22.646	675.52	121.55	451.5	
3	180	6	110	8	110	22.673	698.64	153.83	292.26	
4	140	10	110	8	110	22.464	754.1	123.8	309.29	
5	180	10	110	8	110	22.208	790.44	125.11	294.25	
6	160	8	90	6	110	22.237	712.18	120.64	347.43	
7	160	8	130	6	110	22.809	739.01	137.52	300.3	
8	160	8	90	10	110	22.243	722.45	122.62	339.67	
9	160	8	130	10	110	22.741	748.09	122.45	294.91	
10	160	6	110	8	90	22.674	685.53	140.59	421.55	
11	160	10	110	8	90	22.351	770.72	124.14	301.54	
12	160	6	110	8	130	22.758	688.62	140.54	383.88	
13	160	10	110	8	130	22.388	773.81	124.6	293.77	
14	140	8	90	8	110	22.282	702.44	121.93	376.26	
15	180	8	90	8	110	22.209	732.37	123.05	315.86	
16	140	8	130	8	110	22.826	728.86	121.04	301.25	
17	180	8	130	8	110	22.652	758.39	123.54	293.81	
18	160	8	110	6	90	22.61	724.44	120.41	305.09	
19	160	8	110	10	90	22.559	733.33	122.22	309.18	
20	160	8	110	6	130	22.661	726.75	120.89	295.35	
21	160	8	110	10	130	22.616	737.2	123.05	288.08	
22	160	6	90	8	110	22.237	677.56	119.1	367.52	
23	160	10	90	8	110	22.094	755.55	124.16	325.27	
24	160	6	130	8	110	22.974	696.59	142.05	355.56	
25	160	10	130	8	110	22.455	788.97	124.41	301.89	
26	140	8	110	6	110	22.655	711.15	120.36	362.77	
27	180	8	110	6	110	22.53	740.06	121.12	292.18	
28	140	8	110	10	110	22.623	720	122.22	359.98	
29	180	8	110	10	110	22.468	750.55	123.11	286.47	
30	160	8	90	8	90	22.176	715.75	121.27	349.93	
31	160	8	130	8	90	22.763	742.17	121.26	301.11	
32	160	8	90	8	130	22.298	719.04	122.09	337.27	
33	160	8	130	8	130	22.785	745.06	121.64	294.26	
34	140	8	110	8	90	22.607	714.1	120.97	360.56	
35	180	8	110	8	90	22.473	743.83	121.86	293.59	
36	140	8	110	8	130	22.669	717.19	121.68	361.58	
37	180	8	110	8	130	22.522	746.92	122.4	285.57	
38	160	6	110	6	110	22.728	682.16	136.75	383.55	
39	160	10	110	6	110	22.401	767.35	123.48	300.53	
40	160	6	110	10	110	22.706	691.83	136.78	381.59	
41	160	10	110	10	110	22.341	777.02	125.25	294.14	

Kriging model construction

The Kriging approximation model has the characteristics of high accuracy and high efficiency. Based on the sample points obtained by the Box Behnken method and the calculated response, a Kriging approximate model of the pump truck frame is established. Figure 32 shows a partial three-dimensional response surface.Fig. 32 Partial three-dimensional response surface. (a) X1-X4-P1. (b) X2-X3-P2.

There may be some errors in establishing an approximate model. In order to verify the accuracy of the established approximate model, a deterministic coefficient R2 is introduced. When the value of R2 is closer to 1, the accuracy of the approximate model is higher. In order to verify the accuracy of the established model, 10 sample points are randomly selected to compare the approximate model prediction results with the simulation results from the four aspects: the first-order intrinsic frequency, frame weight, maximum stress value under full-load bending and full-load torsion conditions. The comparison results are shown in Fig. 33. The R2 of the four approximation models are obtained to be 1, indicating that the established approximation models have high accuracy and meet the design requirements.Fig. 33 Precision of approximate model. (a) First order intrinsic frequency. (b) Frame weight. (c) Maximum stress under full load bending condition. (d) Maximum stress under full load torsion condition.

MOGA-based optimization for solving

This study adopts the Multi Objective Genetic Algorithm (MOGA) for optimization solution35,36. Before performing the solution, the number of initial samples is set to 5000, the number of iterative samples is set to 1000, the maximum allowable pareto percentage is set to 70, the convergence stability percentage is set to 2, and the maximum number of iterations is set to 20. After 15,440 evaluations, the multi-objective genetic computation converges and the pareto solution set is obtained as shown in Fig. 34. Each point in the figure represents a candidate point, corresponding to the values of the frame weight and first-order intrinsic frequency. Three final candidate points are selected from these discrete points and the optimization result candidate points are shown in Table 10.Fig. 34 Pareto's solution set.

Table 10 Candidate points for optimization results.

Candidate points	1	2	3	Final dimensions	
X1	157.24	158.83	158.8	158	
X2	7.8451	7.817	7.8569	7.8	
X3	105.86	104.94	103.32	105	
X4	7.4035	7.3352	7.2186	7.3	
X5	104.05	102.48	102.10	103	

Comparison analysis

Modify the frame model based on the final dimensions in Table 10 and perform a new finite element analysis. Compared with the original frame, the optimized emergency rescue mobile pump truck frame has an increase in maximum stress under full load torsion conditions, while the maximum stress values under other working conditions have decreased. The maximum displacement of the frame under the four optimized working conditions does not change significantly compared to the original frame, and the static performance of the frame is good. The first eight constrained modal frequency values of the frame have decreased compared to the original frame, but the amplitude of change is relatively small, with a frequency distribution between 20.558 and 60.571 Hz. The overall frequency distribution can avoid road excitation frequency and diesel engine excitation frequency, and has good dynamic characteristics. At the same time, the optimized size of the frame has a weight of 719.38 kg, which is 87.88 kg lower than the original frame weight and a weight reduction rate of 10.89%, achieving a lightweight design of the frame. The performance comparison of frame before and after optimization is shown in Table 11.Table 11 Performance comparison of frames before and after optimization.

Variable	Original frame	After topology optimization	After size optimization	
Weight (kg)	807.26	730.51	719.38	
Full load bending condition	ω (mm)	1.29	1.32	1.35	
σ (MPa)	126.02	121.88	121.22	
Full load torsion condition	ω (mm)	10.11	11.47	12.56	
σ (MPa)	294.49	295.17	313.49	
Emergency turning conditions	ω (mm)	1.30	1.34	1.36	
σ (MPa)	129.85	126.53	125.98	
Emergency braking conditions	ω (mm)	1.26	1.30	1.32	
σ (MPa)	177.2	167.11	165.46	
Intrinsic frequency (Hz)	First-order	22.031	22.608	22.558	
Second-order	30.453	28.471	28.233	
Third-order	31.646	29.939	29.898	
Fourth-order	40.670	41.154	40.671	
Fifth-order	52.049	46.138	45.697	
Sixth-order	55.016	47.138	46.875	
Seventh-order	59.412	50.246	50.154	
Eighth-order	67.627	65.442	64.571	

Conclusion

A new mobile pump truck frame was designed with reference to the existing mobile vehicle frame model. The materials used are 40Cr and Q235 and are analyzed statically using the finite element method. The static analysis of the original modified design frame shows that under the three working conditions of full load bending, emergency turning and emergency braking, the maximum displacement of the frame is not more than 2 mm, and the maximum stress is not more than 200 MPa. The deformation and stress generated by the frame under full load torsion conditions are relatively large, with a maximum displacement of 10.11 mm and a maximum stress of 294.49 MPa; but they are far below the yield strength limit of the material, which can meet the design requirements for frame strength. However, as the most dangerous working condition, the full load torsional working condition should be avoided as much as possible in actual operation.

After topology optimization, the weight of the frame is reduced by 76.75 kg compared to the original frame, with a weight reduction rate of 9.5%. After topology optimization, the maximum displacement increases and the maximum stress decreases under three working conditions: full load bending, emergency turning, and emergency braking. The maximum displacement and maximum stress under full load torsion condition also increase. However, the changes in maximum displacement and maximum stress under the four classic working conditions are very small. In addition, the first-order intrinsic frequency of the topology optimized frame increases and the eighth-order intrinsic frequency decreases, which further avoids the resonance phenomenon caused by the road surface and the diesel engine. The topology optimized frames can meet the strength design requirements.

After completing topology optimization, use multi-objective genetic algorithm to further optimize the frame. Further optimization of the topology optimized frame using multi-objective genetic algorithm. The optimized frame weight is 719.38 kg, which is 87.88 kg less than the original frame weight and has a weight reduction rate of 10.89%. Under the premise of ensuring the frame design requirements, the lightweight design is realized.

Modal analysis shows that the first-order intrinsic frequency of the frame is 22.03 Hz, which can avoid the resonance phenomenon caused by road vibration; at the same time, the vibration frequency of the diesel engine is 75 Hz, which is higher than the first eight order intrinsic frequency of the frame, and it can also avoid the resonance phenomenon caused by the diesel engine. The harmonic response analysis results show that the peaks of the displacement and stress response curves of the frame model appear near the frequencies of 22 Hz, 40.5 Hz and 59 Hz, and the peaks of the frequency response correspond to the intrinsic frequency of the whole vehicle model, verifying the rationality of the modal frequency response analysis results of the entire vehicle.

Acknowledgements

The research was financially supported by the "Pioneer" and "Leading Goose" R&D Program of Zhejiang (Grant No. 2022C03170).

Author contributions

Yu-Liang Zhang proposed the innovative idea and wrote the manuscript. Hai-Bin Lin carried out the numerical simulation. Zu-Chao Zhu revised the manuscript.All authors reviewed the manuscript and agreed to publish the version of the manuscript.

Data availability

The data that support the findings of this study are available from the corresponding author upon reasonable request.

Competing interests

The authors declare no competing interests.

Publisher's note

Springer Nature remains neutral with regard to jurisdictional claims in published maps and institutional affiliations.
==== Refs
References

1. Qihui L Ben W Zhenqiang Z Damage and failure analysis of hybrid laminates with different ply-stacking sequences under low-velocity impact and post-impact compression[J] Thin-Walled Struct. 2022 180 1 19
Qihui, L. et al. Damage and failure analysis of hybrid laminates with different ply-stacking sequences under low-velocity impact and post-impact compression[J]. Thin-Walled Struct. 180, 1–19 (2022).
2. Veloso V Magalhaes HS Bicalho GI Failure investigation and stress analysis of a longitudinal stringer of an automobile chassis [J] Eng. Fail. Anal. 2009 16 5 1696 1702 10.1016/j.engfailanal.2008.12.012
Veloso, V. et al. Failure investigation and stress analysis of a longitudinal stringer of an automobile chassis [J]. Eng. Fail. Anal. 16(5), 1696–1702 (2009).10.1016/j.engfailanal.2008.12.012
3. Kim D Seo S Kim S Design and performance analyses of thermoelectric coolers and power generators for automobiles[J] Sustain. Energy Technol. Assess. 2022 51 104 116
Kim, D. et al. Design and performance analyses of thermoelectric coolers and power generators for automobiles[J]. Sustain. Energy Technol. Assess. 51, 104–116 (2022).
4. Stellmach S Braun LM Wächter M On load assumptions for self-propelled forage harvesters [J] Int. J. Fatigue 2021 147 1 10 10.1016/j.ijfatigue.2020.106114
Stellmach, S. et al. On load assumptions for self-propelled forage harvesters [J]. Int. J. Fatigue 147, 1–10 (2021).10.1016/j.ijfatigue.2020.106114
5. Bagawan M Krishna MV Kumar PR Design and analysis of electric motorcycle chassis frame [J] Mater. Today Proc. 2023 1 1 7
Bagawan, M. et al. Design and analysis of electric motorcycle chassis frame [J]. Mater. Today Proc. 1, 1–7 (2023).
6. Patel D Jasani V Shah D Design and FE analysis of chassis for solar powered vehicle [J] Mater. Today Proc. 2022 62 3 1626 1631 10.1016/j.matpr.2022.04.137
Patel, D. et al. Design and FE analysis of chassis for solar powered vehicle [J]. Mater. Today Proc. 62(3), 1626–1631 (2022).10.1016/j.matpr.2022.04.137
7. Widiyanto I Sutimin S Laksono FB Structural assessment of monocoque frame construction using finite element analysis: A study case on a designed vehicle chassis referring to ford GT40 [J] Proc. Struct. Integr. 2021 33 27 34
Widiyanto, I. et al. Structural assessment of monocoque frame construction using finite element analysis: A study case on a designed vehicle chassis referring to ford GT40 [J]. Proc. Struct. Integr. 33, 27–34 (2021).
8. Armentani E Giannella V Parente A Design for NVH: Topology optimization of an engine bracket support [J] Proc. Struct. Integr. 2020 26 211 218
Armentani, E. et al. Design for NVH: Topology optimization of an engine bracket support [J]. Proc. Struct. Integr. 26, 211–218 (2020).
9. Gholami J Ghassabi M Optimization and numerical investigation of an excavator carrier [J] J. Terrramech. 2021 97 29 34 10.1016/j.jterra.2021.05.002
Gholami, J. & Ghassabi, M. Optimization and numerical investigation of an excavator carrier [J]. J. Terrramech. 97, 29–34 (2021).10.1016/j.jterra.2021.05.002
10. Mujiburrahman K Saravanakumar S Krishnaraj R Design and analysis of E-glass gear box housing in tractor and optimization of its design parameters [J] Mater. Today Proc. 2022 49 3696 3704 10.1016/j.matpr.2021.10.079
Mujiburrahman, K., Saravanakumar, S. & Krishnaraj, R. Design and analysis of E-glass gear box housing in tractor and optimization of its design parameters [J]. Mater. Today Proc. 49, 3696–3704 (2022).10.1016/j.matpr.2021.10.079
11. Wei W Xinbo C Design methodology for wheel corner module topology based on position and orientation characteristics[J] Mech. Mach. Theory 2019 136 122 140 10.1016/j.mechmachtheory.2019.02.017
Wei, W. & Xinbo, C. Design methodology for wheel corner module topology based on position and orientation characteristics[J]. Mech. Mach. Theory 136, 122–140 (2019).10.1016/j.mechmachtheory.2019.02.017
12. Gautam GD Singh KP Prajapati A Design optimization of roll cage for formula one vehicle by using finite element analysis [J] Mater. Today Proc. 2020 28 4 2068 2076 10.1016/j.matpr.2020.03.052
Gautam, G. D. et al. Design optimization of roll cage for formula one vehicle by using finite element analysis [J]. Mater. Today Proc. 28(4), 2068–2076 (2020).10.1016/j.matpr.2020.03.052
13. Sun T Jiang R Sun H Multiscale uncertainty propagation analysis and reliability optimization of the CFRP crossbeam of the twist beam axle [J] Int. J. Mech. Sci. 2023 242 1 20 10.1016/j.ijmecsci.2022.108022
Sun, T. et al. Multiscale uncertainty propagation analysis and reliability optimization of the CFRP crossbeam of the twist beam axle [J]. Int. J. Mech. Sci. 242, 1–20 (2023).10.1016/j.ijmecsci.2022.108022
14. Mohanavel V Iyankumar R Sundar M Modelling and finite element analysis of anti-roll bar using ANSYS software [J] Mater. Today Proc. 2021 37 321 335 10.1016/j.matpr.2020.05.322
Mohanavel, V. et al. Modelling and finite element analysis of anti-roll bar using ANSYS software [J]. Mater. Today Proc. 37, 321–335 (2021).10.1016/j.matpr.2020.05.322
15. Shengqin Li Xinyuan F Study of structural optimization design on a certain vehicle body-in-white based on static performance and modal analysis [J] Mech. Syst. Signal Process. 2020 135 1 10
Shengqin, Li. & Xinyuan, F. Study of structural optimization design on a certain vehicle body-in-white based on static performance and modal analysis [J]. Mech. Syst. Signal Process. 135, 1–10 (2020).
16. Farahani BV Ramos NV Moreira PMGP Passive safety solutions on transit buses: Experimental and numerical analyses [J] Proc. Struct. Integr. 2022 37 668 675
Farahani, B. V. et al. Passive safety solutions on transit buses: Experimental and numerical analyses [J]. Proc. Struct. Integr. 37, 668–675 (2022).
17. Srivastava JP Chaithanya BK Teja KS Numerical study on strength optimization of Go-Kart roll-cage using different materials and pipe thickness[J] Mater. Today Proc. 2021 39 488 492 10.1016/j.matpr.2020.08.217
Srivastava, J. P. et al. Numerical study on strength optimization of Go-Kart roll-cage using different materials and pipe thickness[J]. Mater. Today Proc. 39, 488–492 (2021).10.1016/j.matpr.2020.08.217
18. Djamaluddin F Optimization of multi cell fender under transverse loading[J] Ocean Eng. 2023 272 1 8 10.1016/j.oceaneng.2023.113740
Djamaluddin, F. Optimization of multi cell fender under transverse loading[J]. Ocean Eng. 272, 1–8 (2023).10.1016/j.oceaneng.2023.113740
19. Kumar A Jaiswal H Ahmad F Dynamic vibration characteristics analysis of truck transmission gearbox casing with fixed constraint of vehicle frame based on FEA[J] Proc. Eng. 2014 97 1107 1115 10.1016/j.proeng.2014.12.389
Kumar, A. et al. Dynamic vibration characteristics analysis of truck transmission gearbox casing with fixed constraint of vehicle frame based on FEA[J]. Proc. Eng. 97, 1107–1115 (2014).10.1016/j.proeng.2014.12.389
20. Hou W Xu X Han X Multi-objective and multi-constraint design optimization for hat-shaped composite T-joints in automobiles [J] Thin-Walled Struct. 2019 143 1 10 10.1016/j.tws.2019.106232
Hou, W. et al. Multi-objective and multi-constraint design optimization for hat-shaped composite T-joints in automobiles [J]. Thin-Walled Struct. 143, 1–10 (2019).10.1016/j.tws.2019.106232
21. Karaoǧlu C Kuralay NS Stress analysis of a truck chassis with riveted joints [J] Finite Elem. Anal. Des. 2002 38 12 1115 1130 10.1016/S0168-874X(02)00054-9
Karaoǧlu, C. & Kuralay, N. S. Stress analysis of a truck chassis with riveted joints [J]. Finite Elem. Anal. Des. 38(12), 1115–1130 (2002).10.1016/S0168-874X(02)00054-9
22. Savkin AN Klimov MA Doluda AO The automobile design element fatigue life modeling due to its dynamic model [J] Proc. Eng. 2017 206 416 420 10.1016/j.proeng.2017.10.494
Savkin, A. N., Klimov, M. A. & Doluda, A. O. The automobile design element fatigue life modeling due to its dynamic model [J]. Proc. Eng. 206, 416–420 (2017).10.1016/j.proeng.2017.10.494
23. Bo L Jian Y Xiaoyu Z Development and application of magnesium alloy parts for automotive OEMs: A review [J] J. Magn. Alloys 2023 11 1 15 47 10.1016/j.jma.2022.12.015
Bo, L. et al. Development and application of magnesium alloy parts for automotive OEMs: A review [J]. J. Magn. Alloys 11(1), 15–47 (2023).10.1016/j.jma.2022.12.015
24. Idrees U Ahmad S Shah IA Finite element analysis of car frame frontal crash using lightweight materials [J] J. Eng. Res. 2023 11 1 1 9 10.1016/j.jer.2023.100007
Idrees, U. et al. Finite element analysis of car frame frontal crash using lightweight materials [J]. J. Eng. Res. 11(1), 1–9 (2023).10.1016/j.jer.2023.100007
25. Sanping Li Hanbin L Yuliang Z Static analysis of mobile pump truck frame for four typical working conditions [J] Appl. Sci. 2023 13 12 1 20
Sanping, Li. et al. Static analysis of mobile pump truck frame for four typical working conditions [J]. Appl. Sci. 13(12), 1–20 (2023).
26. Shimoda M Kameyama K Shi JX Tailoring static deformation of frame structures based on a non-parametric shape–size optimization method [J] Int. J. Solids Struct. 2017 112 143 154 10.1016/j.ijsolstr.2017.02.011
Shimoda, M., Kameyama, K. & Shi, J. X. Tailoring static deformation of frame structures based on a non-parametric shape–size optimization method [J]. Int. J. Solids Struct. 112, 143–154 (2017).10.1016/j.ijsolstr.2017.02.011
27. Majid IA Laksono FB Suryanto H Structural assessment of ladder frame chassis using FE analysis: A designed construction referring to ford AC cobra [J] Proc. Struct. Integr. 2021 33 35 42
Majid, I. A. et al. Structural assessment of ladder frame chassis using FE analysis: A designed construction referring to ford AC cobra [J]. Proc. Struct. Integr. 33, 35–42 (2021).
28. Ekapun P Pang TY Design and performance analysis of an electromagnetic tricycle operated in an airport [J] Proc. Eng. 2015 99 1330 1338 10.1016/j.proeng.2014.12.667
Ekapun, P. & Pang, T. Y. Design and performance analysis of an electromagnetic tricycle operated in an airport [J]. Proc. Eng. 99, 1330–1338 (2015).10.1016/j.proeng.2014.12.667
29. Sanjaya Y Prabowo AR Imaduddin F Design and analysis of mesh size subjected to wheel rim convergence using finite element method [J] Proc. Struct. Integr. 2021 33 51 58
Sanjaya, Y. et al. Design and analysis of mesh size subjected to wheel rim convergence using finite element method [J]. Proc. Struct. Integr. 33, 51–58 (2021).
30. Bertini L Bucchi F Monelli BD Development of a simplified model for the vibration analysis of lawn mowers [J] Proc. Struct. Integr. 2018 8 509 516
Bertini, L. et al. Development of a simplified model for the vibration analysis of lawn mowers [J]. Proc. Struct. Integr. 8, 509–516 (2018).
31. Lang P ANSYS-based soil collection vehicle carriage skeleton study [J] Auto Time 2023 17 134 138
Lang, P. ANSYS-based soil collection vehicle carriage skeleton study [J]. Auto Time 17, 134–138 (2023).
32. Yang L Junzhi Y Di Da Modal analysis of compartment skeleton for the electricity generation car [J] New Technol. New Process 2013 06 20 22
Yang, L., Junzhi, Y. & Di, Da. Modal analysis of compartment skeleton for the electricity generation car [J]. New Technol. New Process 06, 20–22 (2013).
33. Huaizhi Z Jikun Ai Junhui Z Lightweight design of limb leg units for hydraulic quadruped robots by topology optimization and lattice filling [J] J. Mech. Eng. 2024 60 04 420 429
Huaizhi, Z. et al. Lightweight design of limb leg units for hydraulic quadruped robots by topology optimization and lattice filling [J]. J. Mech. Eng. 60(04), 420–429 (2024).
34. Qiang G Jian W Yan Z Topology optimization approaches and its application and prospect in transportation engineering [J] J. Mech. Eng. 2024 60 04 369 390
Qiang, G. et al. Topology optimization approaches and its application and prospect in transportation engineering [J]. J. Mech. Eng. 60(04), 369–390 (2024).
35. Jin H Xiangyu L Pengfei W Multi-objective optimization of a double helical coil heat exchanger using response surface method and genetic algorithm[J] Int. J. Therm. Sci. 2024 199 1 15
Jin, H. et al. Multi-objective optimization of a double helical coil heat exchanger using response surface method and genetic algorithm[J]. Int. J. Therm. Sci. 199, 1–15 (2024).
36. Jianpeng W Yonglin Q Deyou Li Hydraulic optimization of canned-motor pump impeller based on multi-objective genetic algorithm[J] J. Drain. Irrig. Mach. Eng. 2024 42 05 440 447
Jianpeng, W. et al. Hydraulic optimization of canned-motor pump impeller based on multi-objective genetic algorithm[J]. J. Drain. Irrig. Mach. Eng. 42(05), 440–447 (2024).
