Rolling stock manufacturers are finding structural solutions to reduce power required by the vehicles, and the lightweight design of the car body represents a possible solution. Optimization processes and innovative materials can be combined in order to achieve this goal. In this framework, we propose the redesign and optimization process of the car body roof for a light rail vehicle, introducing a sandwich structure. Bonded joint was used as a fastening system. The project was carried out on a single car of a modern tram platform. This preliminary numerical work was developed in two main steps: redesign of the car body structure and optimization of the innovated system. Objective of the process was the mass reduction of the whole metallic structure, while the constraint condition was imposed on the first frequency of vibration of the system. The effect of introducing a sandwich panel within the roof assembly was evaluated, focusing on the mechanical and dynamic performances of the whole car body. A mass saving of 63% on the optimized components was achieved, corresponding to a 7.6% if compared to the complete car body shell. In addition, a positive increasing of 17.7% on the first frequency of vibration was observed. Encouraging results have been achieved in terms of weight reduction and mechanical behaviour of the innovated car body.
1 Introduction
Nowadays, the railway industry moves to eco-sustainable solutions to reduce excessive CO2 emissions and energy consumption [1‐3]. Innovative solutions were proposed to act directly on the vehicle structure, power train system or control system. Harrison et al. [4] presented the development of a detailed MATLAB/Simulink model to control a bimodal train. It combined adaptive speed limit control with selective engine shutdown, reducing the carbon dioxide emissions. Great interest is growing in hydrogen power train systems, widely described from many points of views in Reference [5, 6]. On the other hand, mass reduction of the vehicle structure, through lightweight design approaches [7], could be an important solution to reduce the required power during running operation conditions. It allows the increasing of the payload, reducing at the same time the rail and the wheel wear so that the damage produced on the track by the train [8]. Innovative materials and structural optimization processes represent effective tools for achieving this goal. The car body shell is generally made up of metallic components held together by welds and/or bolts and covered using metallic sheets. In some cases, the structure is made up of aluminium extruded components, which are welded together to create the car body cross section. Grasso et al. [9] proposed three different types of composite panels, tested for innovating a rail vehicle component and carried out an extensive mechanical characterization to assess the mechanical data of lamina. An end car box of a railway vehicle was redesigned introducing carbon fibre composite material [10]. Compared with traditional metallic materials, the weight of the innovated component was about 72% of the weight of aluminium alloy box, maintaining acceptable tensile, fatigue and impact resistance. Pultrusion manufacturing process were investigated for the fabrication of medium-speed railway vehicle mobile panels for the substitution of steel panels, using glass fibre-reinforced polymers (GFRP) [11]. The GFRP fabric pultrusion panel design was successful according to the EN12663-1:2015 and the project requirements, achieving a weight reduction of 35.5% respect to the original design. Yang et al. [12] carried out an experimental and numerical approach for the evaluation of projectile impact behaviour of curved GFRP composites for rail vehicles. Moreover, optimization processes were combined with sandwich structures to improve several different characteristics. With the aim of finding the optimal configuration for composite sandwich structures used in rail vehicle floor panels, in terms of mass and cost, a multiple objective approach was tested [13]. Various requirements, such as stiffness, strength, buckling and thickness were studied to evaluate their influence in the choice of load carrying sandwich panels for high-speed rail vehicles. Then, they were optimized using a finite element (FE) software achieving a mass saving of 30% [14]. The composite body shell of a light rail vehicle was optimized combining shape and size optimization, including 96 constraint functions to select for the single panel, supporting a labour-intensive multi-level approach [15]. Crashworthiness performances of a composite energy-absorbing structure for railway vehicles were optimized by Xie et al. [16]. Finally, optimization process can be applied singularly on car body metallic structures. Topology, shape and size optimization were combined to innovate the ribs of a railway car body shell [17], with the aim of reducing mass. Fatigue life prediction was included in a multidisciplinary design optimization method for lightweight car body [18].
During the present activity, the roof assembly of a light rail vehicle car body has been redesigned for introducing an aluminium honeycomb sandwich panel, using a bonded joint as fastening system. Then, the innovated structure was optimized to reduce the global mass. At this stage of work, the main focus was on the changing in static and dynamic behaviour of the complete redesigned car body, passing from a weld roof structure to a bonded one. Reference European standards for rail vehicle performance evaluation were adopted for testing the car body.
Anzeige
This paper is organized in five sections. In sect. 1, a brief introduction about the application of optimization processes on railway vehicles and some eco-sustainable solutions for car body are included. The proposed methodology is described in sect. 2. The vehicle used as benchmark and the innovation process that involved it are reported in sect. 3. FE structural analysis and application of the optimization approach are explained within sect. 4, where each step has been discussed, including results. Section 5 reports conclusions and future developments of the present activity.
2 Methodology
Methodology includes the following steps. (1) The FE model of the complete vehicle had to be positively verified according to the reference standard EN 12663-1:2015 [19]. Despite the loading conditions were always applied on the whole vehicle, it was important for the reference car body to show a suitable mechanical performance, especially in terms of concentrations of stress and modal behaviour. (2) The reference car body was isolated, including all the necessary elements that affected the dynamic behaviour of the system (i.e. concentrated masses). A modal analysis of the system was made to evaluate its modal behaviour in free–free conditions. First frequency of vibration was then included in the constraint condition used for optimization process. Mode shapes needed to be compared with those of the innovated structure for monitoring possible variations. (3) The car body structure needed to be modified to allow the correct installation of the sandwich panel, according to the fastening system. (4) The redesigned structure was primarily tested with a modal analysis to check possible changing on the dynamic behaviour of the system. Then, their mechanical performances were tested according to EN 12663-1:2015 standard, through static load conditions. (5) The optimization approach was applied on the reference car body with the objective to minimize mass, ensuring the required dynamic behaviour in terms of minimum frequency of vibration. To conclude the verification, the redesigned and optimized structure was tested again statically.
3 Case study—light rail vehicle car body
The light rail vehicle studied in the present work, was a modern tram platform included in P–V category according to the reference standard [19]. It is a monodirectional vehicle composed by five car bodies and three bogies. Two car bodies are suspended type, without direct connection with bogie. Numerical model of the vehicle was built with a commercial FE software. It counted about five million elements, mainly of shell type at first order. Equipment was modelled through concentrated and non-structural masses (NSM).
3.1 Original car body structure
The structure of the car body, as shown in Fig. 1, was totally made with aluminium alloys EN AW 6005 T6 and EN AW 6106 T6, whose properties are described in EN 1999-1-1:2014 standard [20].
Fig. 1
Finite element model of the car body
×
Anzeige
As usual for aluminium car bodies, the main assemblies of the structure were made up and connected exploiting welding process and riveting. At this level of modelling, each rivet was modelled numerically with a simplified approach with the aim of evaluating only axial and shear stresses. They were positioned in the connection interfaces between the upper and lower frame, as indicated by the arrow in Fig. 1. The model counted 140 rivets, uniformly distributed over the four corners of the car body.
The upper panel of the roof, together with the floor panel, thanks to their simple and linear shapes, were considered for introducing the sandwich structure. However, the development of low-floor vehicles has significantly reduced the space for systems positioning, forcing designers to move them to the roof. Due to the increasing number of equipment positioned on the car body roof, this assembly has become fundamental from a structural point of view. Figure 2 shows an isometric view of the upper panel that has been removed from the original roof assembly to allow the introduction of the sandwich structure.
Fig. 2
Replaced upper panel
×
3.2 Car body redesign and sandwich panel modelling
Dealing with the assembly process, the panel had to be positioned from above the pre-assembled welded car body structure. Once the panel was correctly positioned, the bonding agent should be inserted. According to the sandwich panel shape, the suitable geometry for the roof assembly was a simple hole geometry. In fact, without changing the car body geometry and respecting the dimensions of the original components, only one component needed to be adapted for introducing the innovative structure. The starting configuration was an extruded profile with a longitudinally development, while the redesigned one had a rectangular shape, with the same concept of a “circular crown.” Figure 3 illustrates the component before and after the modelling process. It was modelled only with shell elements.
Fig. 3
Redesigned components
×
An aluminium sandwich panel with honeycomb core was selected, thanks to its great mechanical performance in terms of stiffness–mass ratio. Depending on the type of adhesive that was adopted, it could have a service temperature up to 150 °C. In addition, it was totally recyclable with promising performance in terms of fire resistance. Among these the evaluation of the fire behaviour of materials and components, in accordance with European Standard CEI EN 45545-2 [21] with hazard level HL2, was the most challenging to comply.
Sandwich panel was modelled in detail, respecting all the geometrical details. With the aim of streamlining the modelling process, a portion of the honeycomb was created in 3D CAD environment. Then the panel was completed using the tool offered by the FE software. It was modelled totally with shell elements at first order. With the aim of observing potential local deformation effects on the honeycomb core, at minimum two elements should be included in the length along T direction, as stated in Ref. [22]. The adhesive layers between skins and core have been modelled using contact interfaces with freeze option. This condition enforces zero relative motion on the contact interfaces and the gap between them remains fixed at the original value and the sliding distance is forced to be zero. In addition, freeze contact allows to maintain a linear analysis approach and correctly represent the behaviour of the panel and the adhesive, complying with the objective of the present activity. Two types of fastening systems were evaluated: threaded connection and bonded joint. The first option was discarded: the large number of components needed (estimated according to the reference standard [18]) could make the assembly process complex and expensive. An example was represented by the potential coaxiality problems between the holes made on the sandwich panel and the component that would have housed it. In addition, several mechanical discontinuities would be introduced, with possible negative consequences on stress concentrations. On the other hand, bonded joint could make the process simpler, ensuring sealing, contained costs, mechanical strength and good adaptability if distortions or misalignments occur in the structure due to welding process. However, some limitations in terms of maximum temperature, resistance to atmospheric agents and a complex mounting process had to be considered. The introduction of the bonded material to create the joint was the last step of the assembly process. The real process required at first the correct positioning of the panel, maintaining the suitable space between it and the underlying component. Surfaces had to be prepared carefully. The adhesive was placed in this space, in more times and paying close attention to the correct injection times considering the flowing phase and the drying and curing process of the bonding material. The bonding agent was Sikaflex, a versatile one-component polyurethane adhesive/sealant of high quality that cures with exposure to atmospheric humidity. It is widely used as adhesive for the windows assembling in railway vehicles and it was explored for a multi-material application on a light rail vehicle [23]. The bonded joint was modelled with hexa-solid elements. It had a rectangular cross section and it was positioned between the sandwich panel and the redesign component. Table 1 summarizes the main features of the sandwich panel with respect to the FE model and mechanical properties.
Table 1
FE model and mechanical properties of the sandwich panel
Figure 4a shows the bonding joint and its sizing, 4b an extract of the honeycomb core (CAD model) and a partial view of the sandwich panel (FE model) and 4c a global cross-sectional view of the innovated roof.
Fig. 4
a FE model of the bonded joint, b honeycomb and sandwich panel modelling, and c global view of the innovated roof
×
4 FE analysis and optimization process
All the numerical tests were carried out with a commercial FE software. The computer used for the calculation process had the following characteristics: Intel(R) Xeon(R) CPU E5-2643 v4 @ 3.40 GHz, RAM 32 GB. The FE model of the tested car body was composed almost entirely of shell elements. With the aim of testing the mechanical performance of the car body, four loading cases were selected to test the most critical conditions for the vehicle structure (see Table 2) with C0, C2 and C4 conditions as indicated by UNI EN 15663:2019 [26]. Constraint conditions, for all load cases, were represented by an isostatic configuration: the car body is supported vertically at the secondary suspension, laterally at the side pads and longitudinally at the posterior buffers of the cabin.
Table 2
Loading conditions according to EN 12663–1:2015
No.
Loading conditions
Load calculation formula
1
Max vertical load
Vertical load 1.3g· C4
2
Compressive load on the buffers in C0 condition
Vertical load C0·g and longitudinal compressive load on the anterior buffers 200,000 N
3
Compressive load on the buffers in C4 condition
Vertical load C4·g and longitudinal compressive load on the anterior buffers 200,000 N
4
Compressive load on the drawbar in C0 condition
Vertical load C0·g and longitudinal compressive load on the drawbar 100,000 N
4.1 Numerical testing of the innovated car body
The first step after the redesign process was to test the innovated car body evaluating both static and dynamic performances. According to the reference standard, the car body must not be evaluated singularly but considering load conditions applied on the whole vehicle. Results highlighted acceptable values in terms of stress and displacements. The modal behaviour of the single car body was tested through a modal analysis in free–free conditions. First frequency of vibration was 19% higher than the original. An overview of the changes in frequency for the first ten vibration modes is presented in Table 3. In addition, the first mode shape was changed: the first flexural mode that involved the upper panel of the roof, was replaced by a global torsional mode. The comparison is illustrated in Fig. 5. Detailed results will be shown in the next section, including the optimization step. The redesign process resulted in 3% of mass saving respect to the original structure.
Table 3
Frequency comparison for the first ten vibration modes
Mode
Original model (Hz)
Redesigned model (Hz)
Frequency variation (%)
1
11.51
13.75
19.46
2
13.99
14.66
4.79
3
14.24
16.05
12.71
4
16.87
16.45
-2.49
5
20.24
19.64
-2.96
6
20.39
27.91
36.88
7
21.22
31.98
50.71
8
27.96
32.64
16.74
9
29.66
32.76
10.45
10
32.73
34.39
5.07
Fig. 5
Comparison between 1st mode: a original; b redesigned
×
4.2 Optimization process of the redesigned car body
The goal of the dynamic size optimization process proposed by Cascino et al. [27], is to find the minimum value of the thickness that could meet the objective function and the design constraints of the problem. A standard formulation for a structural optimization problem is reported in Ref. [28]. The objective of the process was the mass minimization. Constraint condition was imposed on the minimum frequency of vibration of the complete car body, that must be equal or higher than 13.5 Hz, the minimum value observed in the modal analysis of the redesigned car body. Design variables involved the skins of sandwich panel and the remaining aluminium extruded profiles of the upper panel, as shown in Fig. 6. Thickness changes are illustrated in Table 4 and a general reduction was observed. Minimum values of thickness were imposed all equal to 1 mm with the objective to understand how much the material could still be exploited, considering that thinner and thinner thicknesses could be fabricated thanks to the recent technical improvements for extrusion of aluminium extruded profiles (ALE).
Fig. 6
Cross-sectional view of the innovated roof
Table 4
Optimization process: settings and results
Component
No.
Original thicknesses (mm)
Optimized thicknesses (mm)
Range of variation (max–min) (mm)
Thickness reduction (%)
Lateral extruded
1
Skin 3
1
3–1
66.67
profile (original)
2
Sets 2.8
1
2.8–1
64.29
Medium profile (redesigned)
3
3
1
3–1
66.67
Upper skin (sandwich panel)
4
1
0.5
1–0.5
50.00
Lower skin (sandwich panel)
5
1
0.5
1–0.5
50.00
×
Figure 7 shows the comparison between the first vibration mode of the car body, before and after the optimization process. As expected, little differences can be observed. Focusing on the mass variation of the optimized components, they resulted 63% lighter than the original ones. Table 5 summarizes the results obtained by the modal analysis, referred to the first ten vibration modes of the system. Mode shapes had a very good matching and frequencies have registered an acceptable percentage negative variation, that complied with the mass reduction of the system.
Fig. 7
Comparison between the 1st mode: a redesigned; b redesigned and optimized
Table 5
Frequency comparison for the first ten vibration modes
Mode
Redesigned model (Hz)
Redesigned and optimized model (Hz)
Frequency variation (%)
1
13.75
13.55
− 1.45
2
14.66
14.51
− 1.02
3
16.05
14.69
− 8.47
4
16.45
16.21
− 1.46
5
19.64
17.59
− 10.44
6
27.91
21.59
− 22.64
7
31.98
26.94
− 15.76
8
32.64
29.28
− 10.29
9
32.76
30.21
− 7.78
10
34.39
32.39
− 5.82
×
5 Results discussion
Dealing with the modal behaviour of the innovated car body, Fig. 8 illustrates the comparison between the natural frequencies for the three configurations studied: original, redesigned (introducing the sandwich panel) and redesigned-optimized. An increasing of 17.7% on the first frequency of vibration of the car body was obtained. A general growth in frequency can be observed also for the other modes, except for modes 4 and 5, which have shown a little reduction, without negative effects. In terms of mode shapes, as stated above, there was a change in the first mode shape between the original model and the redesigned one. However, the second mode of the original structure has shown a good matching with the first one of the redesign model. It means that only the first flexural mode referred to the original roof assembly was lost.
Fig. 8
Comparison between the natural frequencies of the three main configurations
×
Once completed the optimization step, the redesigned-optimized version of the model was tested again in accordance with EN 12663–1:2015 standard. All the load cases were applied on the complete vehicle and never on the single car body, as indicated by the reference standard. A lighter car body was designed, achieving a 63% of mass saving for the five components subjected to the optimization approach, which corresponded to 7.6% respect to the whole mass of the car body metallic structure. Through evaluating the global displacement referred to the roof assembly (Fig. 9), a different distribution can be observed. It depends on the great performances in stiffness offered by the sandwich panel: ALE profiles tended to flex in the mean zone of its longitudinal length while the proposed design moves globally in a compact way. Allowing for the displacements along Z direction, the sandwich panel respected the limit value of the inflexion.
Fig. 9
Comparison in terms of displacements of the roof assembly: a redesigned; b redesigned and optimized
×
The reference standard proposes the “utilization coefficient” to evaluate stress concentrations, evaluated as the ratio between calculated stress and permissible stress. Acceptable values must be lower than 1. Table 6 reports the max stress values referred to base material and heat affected material, given the most critical load case conditions. The sandwich panel has shown good performance, with low concentrations of stress located at the end of the skins, probably related to the simplified modelling of the panel and connections. Figure 10a, b illustrates the worst stress concentrations observed in the central pillars of the car body. Figure 11 shows the pressure distribution on the sandwich panel in the max vertical load condition. Some concentrations of stress at the end of the skin were observed, where the constraint to the car body was located. Simplified modelling of the panel allowed to evaluate the global effect on the whole car body, but locally a higher-level modelling will be introduced.
Table 6
Main concentrations of stress resulted in redesigned–optimized configuration
Load case
Component
Material
\({\sigma }_{\mathrm{c},\mathrm{max}}\)(MPa)
\({\sigma }_{\mathrm{amm}}\)(MPa)
U
Max vertical load
1
Base
140.68
200
0.70
2
Heat affected
43.38
115
0.38
Compressive load on the buffers in C4 condition
3
Base
135.89
200
0.68
4
Heat affected
38.16
115
0.33
σc,max is maximum stress evaluated through FE analysis; σamm is permissible stress
Fig. 10
Stress concentrations: a max vertical load for component 1; b compressive load on the buffers in C4 condition for component 3
Fig. 11
Max pressure distribution on the sandwich panel
×
×
In order to complete the verification process on the proposed car body, other aspects were further investigated. The buckling condition for the complete vehicle is tested numerically. The car body structure of a railway vehicle is a complex system that could be subjected to buckling phenomenon locally. Compressive or vertical load conditions are generally tested. In the present activity, two load cases were tested: compressive load on the buffers in C0 condition and max vertical load. The value obtained by the numerical buckling test, was the coefficient to be multiplied to the load to obtain a buckling instability condition. This coefficient, according to EN 12663–1:2015, had to be higher than 1.5. Both loading cases were verified: for the compressive load the coefficient was 2.2, while for the vertical load 1.7. Then, the redesigned car body did not introduce any new local buckling condition. A local buckling mode can be observed in Fig. 12.
Fig. 12
The 1st buckling mode of redesigned-optimized configuration
×
The bonding joint was tested evaluating the stresses and strains on the plane x–y, which had to be lower than reference permissible values. As illustrated in Fig. 13, results highlights that the bonding joint was widely verified, with stress value one order of magnitude smaller than the permissible one.
Fig. 13
Bonded joint Von Mises stresses for max vertical load
×
To conclude, all the rivets of the car body have been tested according to Eurocode 9. For each of them axial and shear forces were calculated and compared with the reference permissible values. Rivets were totally verified.
6 Conclusions
The present activity describes the redesigning and dynamic structural optimization of a light rail vehicle car body, which includes a sandwich panel within the roof structure. The objectives of the authors were the realization of a lighter car body and the evaluation of the global dynamic behaviour of the innovated hybrid system. The optimization approach had the objective to reduce the mass of the car body maintaining its first frequency of vibration sufficiently high. An aluminium honeycomb sandwich panel was tested. It was introduced in the roof assembly of the car body shell and fastened through a bonded joint made with Sikaflex. The first redesign step has shown a changing in the first mode shape of the car body, replacing the first flexural mode referred to the upper panel of the roof with a global torsional mode which involved the whole car body. In terms of frequency, an increasing about 20% was obtained for the first one. Optimization process also involved the sandwich panel. The optimized components have shown a mass saving of 63%, that corresponded to a 7.6% if referred to the whole car body. Despite the weight reduction of the system, the new dynamic conditions were suitable, with a final first frequency equal to 13.5 Hz. In terms of mechanical performance, the metallic structures of the car body did not show any problems, with utilization coefficients widely lower than 1. The same results were achieved for rivets and bonded joint. The optimized configuration of the sandwich panel highlighted an acceptable behaviour in terms of inflexion, respecting permissible values. A higher-level modelling of it will be made to evaluate local mechanical behaviour more specifically. This point will be further investigated. To conclude, the presence of the sandwich panel caused a positive impact on the dynamic behaviour of the system, widening the gap respect to the minimum acceptable frequency of vibration for a light rail vehicle car body. In addition, a lighter structure was obtained, with acceptable mechanical performance. Even if these preliminary results are encouraging, much work remains to be done with the aim of making the optimization process more effective for local stress effects. Moreover, a detailed modelling for sandwich panel and bonded interfaces will be proposed in our future work.
Open Access This article is licensed under a Creative Commons Attribution 4.0 International License, which permits use, sharing, adaptation, 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 changes were made. 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/4.0/.
