Design analysis and optimization of the Hyperloop shell and chassis
Fangzhou Shao
Master of Science Thesis TRITA-ITM-EX 2019:564 KTH Industrial Engineering and Management
Machine Design SE-100 44 STOCKHOLM
1 Examensarbete TRITA-ITM-EX 2019:564
Designanalys och optimering av Hyperloop-skal och chassi
Fangzhou Shao
Godkänt
2019 -08-28
Examinator
Ulf Sellgren
Handledare
Moeen Rajput
Uppdragsgivare Daniele Piva
Kontaktperson
Moeen Rajput
Sammanfattning
Ett Hyperloop-system utvecklas för närvarande av Integrated Transport Research Lab (ITRL) vid KTH Royal Institute of Technology för att delta i den kommande Hyperloop Pod-tävlingen. Hyperloop-gruppen vid KTH har utvecklat en primärkonstruktion av chassi och skal. De har dock ingen aning om hur bra deras nuvarande design är. Eftersom hastigheten är de enda kriterierna för denna tävling, vill de också minska massan så mycket som möjligt. I detta avseende är det nödvändigt med finita element- och optimeringsanalyser.
Syftet med denna masteruppsats är att analysera den aktuella skal- och chassikonstruktionen för att utvärdera kvaliteten på dess fästen och integriteten hos designen, samt att minska den totala massan samtidigt som styvheten uppfyller specificerat krav. De använda verktygen är HyperMesh, Optistruct och HyperView som är delar av programvaran HyperWorks från Altair.
Nyckelord: FE-analys, formoptimering, optimering av topologi, optistrukt, kompositmaterial
2
3
Master of Science Thesis TRITA-ITM-EX 2019:564
Design analysis and optimization of the Hyperloop shell and chassis
Fangzhou Shao
Approved
2018-08-28
Examiner
Ulf Sellgren
Supervisor
Moeen Rajput
Commissioner
Daniele Piva
Contact person
Moeen Rajput
Abstract
In the past decades of years, huge amounts of people chose to move to big cities for better education and medical service, which also makes many cities are very crowded and noisy. Moreover, the house rent in city center is some kind too expensive for many people, especially for the youth. In this sense, more people are willing to live in suburb instead of city center. Due to the larger distance between home and office, people’s requirement for a faster public transportation method is enormous.
Elon Musk first publicly mentioned the concept of Hyperloop in 2012[1], which is a sealed tube or system of tubes with nearly vacuum condition through which a pod can transport people or objects at super high velocity. With the linear induction motor and magnetic levitation technology, the drag force on the pod can be reduced tremendously, thus increasing the peak velocity to 1200 km/h. To gather more ideas for this concept, SpaceX holds the Hyperloop Pod Competition where worldwide teams will design their own Hyperloop pod to demonstrate their technical feasibility of new ideas [2].
A Hyperloop system is currently in development by the Integrated Transport Research Lab (ITRL) at KTH Royal Institute of Technology to participate in the upcoming Hyperloop Pod Competition. KTH Hyperloop group has some primary design of chassis and shell. However, they have no idea how good of their current design is. Furthermore, since the velocity is the only criteria for this competition, they also want to reduce the mass as much as possible. In this sense, some finite element analysis and optimization analysis are necessary.
The objective of this master’s thesis is to analyze the current shell and chassis design to assess the quality of the attachments and integrity of the design and to reduce the total mass while keeping the stiffness within the safety range. The used tools are HyperMesh, Optistruct and HyperView which are parts of the software HyperWorks from Altair.
Keywords: FE analysis, shape optimization, topology optimization, Optistruct, composite material
4
5
FOREWORD
This master’s thesis is the final part of the master’s program in Engineering Design, Machine Design track at Royal Institute of Technology. This thesis is carried out from February to July 2019 at the office of Sigma Industry.
I would like to thank everyone who has helped me in this Master’s thesis work.
Firstly, I would like to thank my supervisor at Sigma Industry, Moeen Rajput, for his patience and guidance during the thesis work. His comments and instructions have saved me a lot of time to learn a new software and keep me in the correct direction.
Secondly, I would like to thank all group members in Simulation & Analysis group in Sigma Industry, especially the group leader, Daniele Piva. They all are experienced analysts and gave me a lot of ideas and suggestions for my thesis work. Moreover, I would like to thank my supervisor and examiner at Royal Institute of Technology, Ulf Sellgren, for his suggestions and comments.
I want to express my thankfulness to Altair Engineering for providing me with the license of the software and very useful online lessons so that I can complete my thesis work.
Finally, I am thankful to all the group member in KTH Hyperloop group. Their enthusiasm and hard work motivate me a lot.
Fangzhou Shao Stockholm, August, 2019
6
7
NOMENCLATURE
Use 12 pt Times New Roman, Italic and 6 pt before and 12 pt after, to describe the content of this chapter in two or three justified rows, e.g. Here are the Notations and Abbreviations that are used in this Master thesis. (Only include the lists that are applicable). The lists are written in 12 pt Times New Roman, 6 pt before.
Notations
Symbol Description
𝜎1𝑡_𝑢 Tensile strength in zero-degree 𝜎1𝑐_𝑢 Compression strength in zero-degree
𝜎1 Stress in zero-degree
𝜎2𝑡𝑢 Tensile strength in 90-degree 𝜎2𝑐_𝑢 Compression strength in 90-degree
𝜎2 Stress in 90-degree
𝑆 Shear strength
𝜀1𝑡_𝑢 Max tensile strain in zero-degree 𝜀1𝑐_𝑢 Max compression strain in zero-degree
𝜀1 Max strain in zero-degree
𝜀2𝑡𝑢 Max tensile strain in 90-degree 𝜀2𝑐𝑢 Max compression strain in 90-degree
𝜀2 Max strain in 90-degree
𝜀12_𝑢 Max plane strain
𝜀12 Plane strain
𝐹12 Normal interaction term in Tsai-Wu failure theory
Abbreviations
CFD Computational Fluid dynamics
FEM Finite Element Analysis
8
TABLE OF CONTENTS
SAMMANFATTNING (SWEDISH) 1
ABSTRACT 3
FOREWORD 5
NOMENCLATURE 7
TABLE OF CONTENTS 9
1 INTRODUCTION 11
1.1 Background 11
1.2 Purpose 11
1.3 Delimitations 12
1.4 Method 12
2 FRAME OF REFERENCE 13
3 IMPLEMENTATION 15
4 RESULTS 17
5 DISCUSSION AND CONCLUSIONS 19
5.1 Discussion 19
5.2 Conclusions 19
6 RECOMMENDATIONS AND FUTURE WORK 21
6.1 Recommendation 21
6.2 Future work 21
7 REFERENCES 23
APPENDIX A: SUPPLEMENTARY INFORMATION 25
9
10
1 INTRODUCTION
This master’s thesis is about the design, analysis and optimization of the chassis and shell of the Hyperloop pod. The background, the purpose, the limitations and the method(s) used will be described in this chapter.
1.1 Background
The Hyperloop transport concept was proposed by Elon Musk in the Hyperloop White Paper published in 2012. This system was introduced with the goal of combining cutting-edge engineering technologies to create the fifth mode of transportation. By utilizing a low-pressure tube as the operation environment and implementing magnetic levitation, the drag forces exerted on the vehicle can be reduced dramatically which would facilitate achieving a peak velocity of 1200m/s.
The Hyperloop Pod competition is a competition sponsored by SpaceX where worldwide teams will gather together to show their own Hyperloop pods to demonstrate the feasibility of the new ideas about Hyperloop concept. All pods are judged only on one criteria: maximum velocity with successful deceleration i.e. without crashing.
There are two key rules according to the Hyperloop Competition Rules and Specification. One is that all teams have to use their own communication system. The other is Pods must be designed and tested to propel themselves to within 100 feet of the far end of the tube before stopping.
An Hyperloop system is currently in development by the Integrated Transport Research Lab (ITRL) at KTH Royal Institute of Technology to participate in the upcoming 2020 Hyperloop Pod Competition. To design the Hyperloop vehicle, knowledge from different fields like aerodynamics, control theory and magnetic physics should be gathered and put into practice. The competition will take place in July and most design work has been done. However, there still exist great possibilities to improve the performance of both shell and chassis.
1.2 Purpose
Although the chassis and shell have been designed, the structure analysis for these parts have not been done. The current design of chassis and shell should be analyzed in finite- element analysis to get the stress distribution and deformation under different load conditions, including lifting, acceleration and braking processes. Only when analysis results are available, KTH Hyperloop can check whether the current designs are qualified or not.
Moreover, since the only judging criteria of Hyperloop Pod Competition is to reach the maximum speed with successful deceleration. Apparently, the whole vehicle should be as light as possible to reach a higher velocity. In this sense, optimization should be done to reduce the weight of the shell and chassis parts as much as possible to increase the peak velocity that the pod can reach.
The current thesis project will be done in collaboration with Sigma Industry East North and KTH Hyperloop team.
11
1.3 Delimitations
It is good practice to define and describe limitations of the project/task in the introductory chapter.
● Only chassis and shell design should be analysed
● Available material should be figured out by structure group in KTH Hyperloop
● The validation of the final design in reality test will be not within the scope
● 70% of finite element analysis and 30% of design
● Vibration and response analysis will not be part of the scope
● The simulation will be based on the current design. Any changes from KTH Hyperloop on the current design will not be taken into consideration.
1.4 Method
The thesis work can be divided into three parts: Literature review and research, analysis for chassis and shell, optimization for chassis and shell.
The first part is the literature review and research, including reading the material about the Hyperloop concept and Hyperloop Pod Competition so that I can have a basic understanding of the rules and constraints for my future design. Reading the final reports from other groups in past few years’ competition can also help to generate some new ideas to reduce the weight and increase the stiffness. Moreover, some research articles about the simulation and optimization are necessary. The general methodology to conduct the analysis and optimization from these articles can make the work more efficient. The literature research also contains the time to learn how to use the software, including how to do the inertia relief analysis and how to do the optimization analysis and what’s the correct steps for optimization.
The second part is the analysis for the chassis and shell that are made of aluminum and carbon fiber respectively. Three loading cases of lifting, braking and acceleration should be conducted and we can get the displacement, strain and stress of all components to check whether the performance of current design is good.
The final part is the optimization for the chassis and shell and generation of the new design. According to simulation results from the second part, the critical areas on the chassis and shell can be figured out. According to the results of size and topology optimization analysis, some unnecessary parts can be removed while the critical parts should be enhanced.
12
13
2 FRAME OF REFERENCE
The reference frame is a summary of the existing knowledge and former performed research on the structure analysis and optimization analysis on metal and composite material. This chapter presents the theoretical reference frame that is necessary for this thesis project.
2.1 Finite Element Analysis
Finite element analysis uses mathematical approximation to simulate real physical systems. With simple and interacting elements, a finite number of unknowns can be used to approximate a real system with infinite unknowns.
Finite element analysis is to solve complex problems with simpler problems.
Because the actual problem is replaced by a simpler problem, this solution is not an exact solution, but an approximate solution. Since most practical problems are difficult to obtain an accurate solution, finite element analysis is time-saving, highly accurate with proper element number, and adaptable to various complex shapes, thus becoming an effective engineering analysis tool. Finite element analysis is used widely in structure analysis, heat transfer, mass flow, electromagnetic potential and so on [3].
The concept of finite element has been produced and applied centuries ago, for example, using a polygon to approximate the circle to find the circumference of the circle.
There are many types of analysis that are used under different conditions. The two most common methods are static analysis and Inertia relief analysis.
2.1.1 Static Analysis
Static analysis is the simplest and most common analysis in engineering fields, which is used to determine the stress, strain, displacement and forces in structures with external loads. When conducting linear static analysis, external forces, pressure, acceleration forces and constraint points should be specified.
Figure 1. Example of FEM static analysis [4]
14
2.1.2 Inertia Relief Analysis
Inertia Relief analysis is applied to the system that is not fully constrained or moves at a long distance. The linear static analysis requires that the system is constrained, or the singularities will occur in the stiffness matrix, making the results invalid.
When conducting inertia relief analysis, the external loads will be balanced by a set of translational and rotational accelerations instead of traditional reaction forces.
One example is the satellite in the aerospace, which gets the external propulsion force from the engine and moves at a long distance in the space without constraints. Then, the inertia relief analysis is necessary to calculate the stress, strain and so on.
Since the Hyperloop will run along the tube, the inertia relief analysis should be applied for the braking and acceleration process.
2.2 Structure Optimization
The purpose of the structure optimization is to find the optimal material distribution to achieve some given objectives under certain limitations or requirements. Some common objectives are to minimize the weight, minimize the cost or increase the rigidity of the structure.
This optimization process is an iterative process. The first step is to think of a design. The second step is to evaluate whether the requirements or limitations are satisfied or not through finite element analysis. If it’s fulfilled, the optimization is determined. If not fulfilled, new changes should be made and repeat the previous steps.
In this sense, the time spent on the optimization process depends on how much extent the designer wants to improve the original design. In most cases, optimization takes quite a long time and the result depends heavily on the designer’s knowledge and experience.
Figure 2. Difference between size, shape and topology optimization [5]
2.2.1 Size Optimization
Sizing optimization is the simplest form of structural optimization. The objective is to optimize the structure by adjusting sizes of the components like thickness of the component and so on. When optimizing the composite materials, size optimization will be conducted to determine the most suitable thickness of plies. Thus, it can help engineers to reduce development time of products made of composite materials.
15
2.2.2 Shape Optimization
In shape optimization, the purpose is to adjust the shape and inner boundary dimensions of the structural design to find the optimal geometry of the structure to achieve customer requirements like minimizing the weight and so on.
2.2.3 Topology Optimization
The most general form of structural optimization is topology optimization. The purpose is to find the optimum distribution of material.
With topology optimization, the optimal material distribution can be found in the design space of uniformly distributed materials to achieve some objectives. Compared with size and shape optimization, topology optimization has more design freedom than other two optimization methods, which is one of the most promising aspects of structural optimization.
2.3 Composite Material
Composite materials are new materials that is made of a combination if two or more different materials to optimize the combination of material components of different properties. The history of composite use can date back to ancient times. The straw- reinforced clay that has been used to build houses in ancient ages and the reinforced concrete that has been used for hundreds of years are two typical composite materials.
Since composite materials are used widely in high-tech fields like aerospace and military due to its high stiffness, high tensile strength, low weight, high chemical resistance, high temperature tolerance and low thermal expansion, composite materials are more and more important in the development of modern science and technology.
The development of the composite material has become one of the most important indicators to measure the advanced level of science and technology in a country.
A generally defined composite material must meet the following conditions [6]:
● Composite materials must be man-made and designed and manufactured according to the requirements;
● Composite materials must be composed of two or more chemically and physically different material components. There should exist some distinct interfaces between the components;
● Composite materials not only maintain the advantages of the properties of the various components, but also achieve the comprehensive properties that cannot be achieved with a single constituent material
2.3.1 Laminate Theory
A ply, or a lamina, is a single layer of a composite material which consists of fibres embedded in matrix [7]. To define the material characteristics of a lamina, three orthogonal axes are established as length (L), width (W) and transverse (T).
There are mainly four different laminae as shown in Figure 3. The first type is unidirectional, where the fibers are placed in the same direction in the lamina. The
16 second type is bi-directional, where the fibers are commonly placed in two perpendicular directions in the lamina. The third type is discontinuous fiber, where the discontinuous fibers are placed in random directions. The final one is woven fiber, which is quite similar to bi-directional fibers.
Figure 3. Different kinds of plies [7]
To form a laminate, several plies will be assembled together as shown in Figure 4.
Figure 4. Laminate example [8]
2.3.2 Failure Modes in Composite Materials
Dislike the steel and aluminum, the failure modes of carbon fiber are quite complicated since carbon fiber is orthotropic instead of isotropic. The failure is caused by different loading conditions. In this sense, we will divide the failure modes according to the load types as tensile failure, compressive failure and interlaminar failure.
17 Tensile failure implies that the fracture in laminate is caused by the tensile forces. There are two conditions that the tensile force is longitudinal to the fibers or transverse to the fibers. For a unidirectional lamina, if the longitudinal loads cause the fracture, it is a fibre dominated failure mode. If it is transverse loads that cause the fracture, it is matrix dominated failure mode.
Actually, these concepts are quite easy to understand. Since the lamina is super strong along the fiber direction and quite weak in the transverse direction, the fiber will contribute more to the whole stiffness in the longitudinal direction and the matrix will contribute more to the whole stiffness in the transverse direction.
Compression failure implies that the fracture is caused by the compression forces. When the compression load applied on the laminate increases, the fibers will bend, thus causing fracture.
The interlaminar failure is due to transverse normal stresses, transverse shear stresses or even in compression. The interlaminar failure will cause delamination between plies or fiber/matrix interface failure.
Figure 5. Failure modes of the composite materials [9]
2.3.3 Composite Material Failure Theory
Lamina failure theories can be classified in three catalogs [10]:
1. Non‐interactive or limit theories: failure is determined by comparing lamina stresses or strains with corresponding ultimate strains or strengths. The limitation is that the interaction between stress components are not taken into consideration.
Examples of such theories are maximum strain criteria and maximum stress criteria.
2. Interactive theories: overall failure can be predicted by one failure criteria that includes all stress components and their interaction. The limitation is that the failure mode cannot be figured out. Examples of such theories are Tsai-Wu criteria and Tsai-Hill criteria.
3. Partially interactive or failure-mode-based theories: different failure criteria will be applied to the failure of matrix, fiber and interface, which is close to the reality.
Examples of such theories are Hashin failure criteria and Puck failure criteria Maximum Stress Criteria:
−𝜎1𝑐_𝑢 < 𝜎1 < 𝜎1𝑡_𝑢
−𝜎2𝑐_𝑢< 𝜎2 < 𝜎2𝑡_𝑢
|𝜏12| < 𝑆
18 Maximum Strain Criteria:
−𝜀1𝑐_𝑢 < 𝜀1 < 𝜀1𝑡_𝑢
−𝜀2𝑐_𝑢 < 𝜀2 < 𝜀2𝑡_𝑢
|𝜀12| < 𝜀12_𝑢 Tsai-Hill Criteria:
𝜎12
𝜎1_𝑢2− 𝜎1𝜎2
𝜎1_𝑢2 + 𝜎22
𝜎2_𝑢2+ 𝜏122 𝜏12_𝑢2 = 1 Tsai-Wu Criteria:
𝜎12
𝜎1𝑐_𝑢𝜎1𝑡_𝑢+ 𝜎22
𝜎2𝑐_𝑢𝜎2𝑡_𝑢 + 𝜏122
𝜏12_𝑢2+ 2𝐹12𝜎1𝜎2+ 𝜎1
𝜎1𝑡_𝑢− 𝜎1
𝜎1𝑐_𝑢+ 𝜎2
𝜎2𝑡_𝑢− 𝜎2 𝜎2𝑐_𝑢 = 1
19
20
3 IMPLEMENTATION
In this chapter, the working process is described. A structured process is often called a method and its purpose is to help to reach the goals for the project. Requirements should be figured out at the beginning of the project. According to these requirements, the concept can be generated.
3.1 Requirements Specification
As this project aims to reduce the weight of chassis and shell while increasing the stiffness, structure analysis and optimization analysis should be developed. With these analysis results, new design can be generated. In this section, the requirements needed to be fulfilled will be listed.
3.1.1 Feature
After understanding of the Hyperloop concept and discussing with the KTH Hyperloop group, the feature requirements for shell and chassis are finalized as shown below.
● Easy to install
● Robust to finish the competition
● Rigid to hold all components
● Easy access for maintenance
● Safe to handle
● Light to increase the peak velocity
3.1.2 Hyperloop Pod Competition Requirements
According to Hyperloop competition rules and requirements, the pod should move on the I-shape beam in the tube provided by SpaceX. In this sense, there are some constraints for
Figure 6. Tube and I-shape beam dimension [11]
21 Table 1.Competition constraints
Pod constraints Tube constraints:
Mass < 1500 kg Outer diameter: 72 in
Length dimension: 5-14 feet Inner diameter: 70.6 in
Safety factor > 2 Length: 1.25km
Internal P: 0.125-14.7 PSI Concrete height: 10.4 in
Since the components including the friction braking system, current braking system, electronic system and etc. are finalized, the corresponding intersection parts should be maintained.
Moreover, the friction braking pad and I-beam should always be in contact, or the friction braking system will not work. In this sense, another requirement is that the displacement of the friction braking system in transverse direction cannot be over 2 millimeters.
3.2 Pod Design Description
Before working on the simulation, the interfaces between chassis and the other components should be figured out so that we can know how to model the structure and how to apply the boundary conditions.
Understanding the basic functions and positions of all components are the first step of the analysis. There are five main systems in the pod [12]:
● Propulsion System: Double Sided Linear Induction Motor (DSLIM) is used to provide the propulsion forces to the Pod
● Braking System: The Eddy current brake system and friction brake system are used to generate a total deceleration force of 6000N to stop the pod safely without crashing.
● Levitation System: The magnetic levitation system will be placed on the skis and connected to the chassis to lift the pod from the ground, thus decreasing the friction force.
● Electronics System: Electronics system will collect the sensor data to controll and monitor the system. Electronics system will be also used to transfer the data to the laptop and receive the orders from laptop remotely.
● Control and Navigation System: The navigation and control system will report the current state of the pod and the performance of all components.
In Figure 7, it demonstrates the chassis with some other systems fixed on it. There is one battery box placed on the top of the chassis, where the electronics system and control and navigation system will be fixed on the battery box. On the right side in the figure is the front face of the chassis and the rear face is on the left side. There are one friction braking system and one Eddy current braking system fixed on the sides of the chassis in both front and rear parts. Two groups of linear induction motor are fixed in the central of the chassis. Each group will attach to one side.
22 Figure 7. Chassis with some other systems
The exploded-view drawing of the KTH Hyperloop pod design in figure 6 shows more information about the position of different components.
From the top-down version, the first one is the carbon fiber shell, following by the electronic system and battery box, chassis with braking systems and motor and skis with magnetic levitation system. Two components not mentioned in last paragraph are the shell and skis with magnetic levitation system. The shell acts like a cover to reduce the drag force on the whole pod. The skis are on the two sides of the chassis and they will be connected with the beams and the sides of the chassis. There will be some springs between the beams and skis, like the shock absorb to exclude the vibration on the chassis.
Figure 8. Exploded-view drawing of KTH Hyperloop pod design
There are three loading cases to be conducted. The first one is lifting. Before starting up the pod, four group members need to lift the pod to the tunnel and then run it. The second one is braking. To finish the competition, all pods should stop
23 successfully without crashing in the tunnel. Two friction braking systems and two Eddy current braking systems are placed on the chassis. There will exist normal and friction forces applied on the chassis. To check whether these forces will cause the failure on the chassis, braking process should be analyzed. The third loading case is acceleration.
At the beginning of the competition, the pod will accelerate to the peak velocity.
Similarly, the forces from the motor should also be analyzed.
The masses of different subsystems are listed in Table 2.
Table 2. Masses of subsystems
Subsystem Mass (kg)
DSLIM 68.00
Ski (2x) 55.99
Eddy current braking (2x) 47.38
Friction braking (2x) 21.48
Chassis 23.104
Battery system 73.95
Lateral stability module (2x) 5.212
Shell 6.1
Inverter 15
Low voltage battery (2x) 1.656
Electronics and sensors 5.1
After understanding the structure of the pod and how it works, chassis can be modeled in the Hypermesh.
First, the STEP file of the chassis should be imported to the Hypermesh and click the function that splits the component by body. Then we can get the 3D model of the whole chassis as shown in Figure 9.
Figure 9. CAD file of the chassis part
24 Second, midsurface of all components will be constructed. Since the chassis is made of sheet aluminum, it can be modeled with shell elements, which is 2D elements.
Using 2D elements instead of 3D element can save huge amounts of time. Moreover, since the chassis is symmetrical with XZ plane, we can keep only half of the model and add some so-called “symmetric constraints” to make the half model perform as the whole model. As shown in Figure 10, all the nodes on the symmetric axis should be constrained on DOF 2,4,6 to make it perform as the whole model.
Figure 10. Chassis model with symmetric constraints
Contact surfaces and type of contact will be used to define the relationship between the components to unit all the components as a whole pod. Since the goal is to assess the performance of the current chassis design, tie contact is chosen, which simplifies the model and saves quite a lot time. The contact relationship is shown in Figure 11.
Figure 11. Contact relationship between surfaces
Next, mass nodes should be used to represent the components attached to the chassis as shown in Figure 12. Components including two braking systems, skis, battery box, electronic system and motor will all be connected to the chassis to get as close as possible to the reality world. 1D element, RBE3, is used to connect the nodes of
25 connection parts and mass nodes because RBE3 will not affect the stiffness of the structure. The light blue parts are all RBE3 elements.
Figure 12. Chassis model with all mass nodes
After that, forces can be applied on the mass node of the components. For example, since the friction force occurs at the connection point between I-beam and friction braking pad, the friction force should be added on the mass node of friction braking system.
Finally, material and property should be assigned to the whole chassis in Hypermesh. The thickness of all shell elements is 3 mm according to the structure group in KTH Hyperloop. Necessary inputs of aluminum property from chosen supplier is listed in Table 3.
Table 3. Material property of aluminum
Young’s Modulus 75000 MPa
Poisson’s Ratio 0.33
Density 2790 kg/m3
Yield Stress 240 MPa
Yield Strain 0.2%
Shell Modeling
Since the shell from the CAD file designed by the aerodynamic group in KTH Hyperloop is just the combination of some surfaces, we can mesh these surfaces directly after importing the STEP file.
26 Figure 13. Shell model of 2D elements
The shell is made of composite material, carbon fiber. For carbon fiber, some plies are first to be created and then construct the laminate with these available lies created before.
The laminate should be quasi isotropic, balanced and symmetric, or the laminate will suffer some twisting torque even though there are no external forces applied on it.
The laminate is shown in Figure 14 as [0/45/90/−45]𝑠.
Figure 14. Laminate of the shell
The thickness of all plies is 0.3 mm because of the minimum thickness that the chosen supplier can manufacture is 0.3 mm. The zero-direction of ply is along z-axis in Figure 15.
Figure 15. Laminate with fiber direction
27 The type of carbon fiber is T700s, whose property is shown in Figure 16. The density of this type of carbon fiber is 1540 kg/m3.
Figure 16. T700s carbon fiber property [13]
3.3 Overall Concept Generation
To increase the stiffness and reduce the weight of the chassis, structure analysis and optimization analysis are integral. There are some steps to conduct the simulation for chassis made of aluminum. One thing to keep in mind is to make the simulation as close to the reality as possible.
The first step is to understand how the current pod work. All other components including battery box, electronic and control system, ski and magnetic levitation system, friction braking system, Eddy current braking system and pod stability system will be fixed on the chassis, so the connection parts between the chassis and these components must be maintained. Meanwhile, the loading cases and corresponding boundary conditions like forces from these components and constraints will be clear.
The second step is to run the simulation of structure analysis on the HyperWorks with all loading cases. After checking the displacement, strain and stress from the simulation results, the performance of the current chassis design can be resolved.
The third step is to run the optimization on the HyperWorks. With structure optimization results, we can check the how different components contribute to the whole stiffness. The parts with higher element density implies that they contribute more to the stiffness and should not be removed. Also, the size optimization gives the optimized thickness for each component with the given constraints.
According to the structure analysis and optimization results, some unnecessary parts that contribute almost nothing to the whole stiffness can be removed and the thickness of the components can be reduced for some non-critical parts, thus reducing the mass as much as possible.
28 For shell part, the procedure is quite similar to the chassis part. Since the shell is made of carbon fiber that is a composite material, the failure mode and criteria are totally different from the isotropic materials like aluminum and steel. In this sense, the first step is to do some information research.
The second step is to run the structural simulation on the HyperWorks with given loading cases. By checking different composite failure criteria, the performance of the current shell design can be figured out.
The third step is to do the optimization to reduce the weight of the shell part.
Through free size optimization, size optimization and shuffle optimization, new design can be finalized. After understanding the most efficient way to do composite material optimization, some noncritical parts in the chassis can be replaced by carbon fiber to reduce more weight.
Except for the changes from the structure analysis and optimization analysis results, alternative material and structure can also be taken into consideration.
For chassis, using carbon fiber sandwich with an aluminum honeycomb core instead of solid aluminum can reduce the weight a lot. This honeycomb sandwich material has high stiffness with low density. The drawback of this honeycomb structure is that it needs specific mounting parts different from the traditional ones as shown in Figure 2. Moreover, the whole chassis can be manufactured by carbon fiber. Carbon fiber is really expensive and its fault tolerance is really low that once some parts of the carbon fiber chassis are broken, it’s not possible to repair them. However, the weight of chassis can be reduced enormously due to the low density and high stiffness of carbon fiber. Besides, some high-stiffness materials like high strength steel can be used on critical parts so that other parts’ thickness can be decreased.
Figure 17. carbon fibre sandwich with an aluminum honeycomb core [14]
29 Figure 18. Mounting for carbon fiber sandwich with an aluminum honeycomb core [15]
From the aspects of structure, uniting the components as a whole body can be practical. Since there are a lot of components in the current design of chassis, the weight of connection parts and weld material occupies quite a large percentage of the total weight. Hence, uniting some of these components is a possible solution. Alternatively, components like battery box can be made as part of the chassis to increase the stiffness.
30
31
4 RESULTS
In the results chapter the results that are obtained with the process/methods described in the previous chapter are compiled, and analyzed and compared with the existing knowledge and/or theory presented in the frame of reference chapter.
4.1.1 Lifting case
Since there are many components connected to the chassis, mass nodes are used to represent these components and they are connected to the nodes of the corresponding connection areas by 1D element, RBE3. However, since the forces from the battery box and electronic system contribute uniformly on that area, pressure should be applied on that area instead of mass node.
The areas where people hold the pod should be constrained in z-axis (DOF 3) as shown in Figure 19 and gravity field should be applied to the whole system. The thickness of the whole chassis is 3 mm and the material is aluminum.
Figure 19. Chassis model with constraints in lifting case
Since the yield stress for the aluminum is 240 MPa and the safety factor should be over 2 according to the competition rule, the maximum von-Mises stress in the chassis should be less than 120 MPa.
According to the simulation, the displacement and von-Mises stress of the lifting loading case are shown in Figure 20 and Figure 21. The part with red color implies that the stress there will be over 120 MPa and displacement is over 2 millimeters, which will cause failure. Since there are no red points in Figure 20 and 21, there won’t exist failure in the chassis. The maximum stress in lifting case is 72.26 MPa.
Thus, current chassis design’s performance in lifting case is good enough.
32 Figure 20. Displacement of chassis in lifting case
Figure 21. Stress of chassis in lifting case
4.1.2 Braking case
Similar to lifting case, mass nodes are used to represent the components and connected to the nodes of the corresponding connection areas by 1D element, RBE3. The only difference is that we use the mass node and apply the gravity to it to represent the battery box instead of pressure force because we use the inertia relief analysis, where the applied loads will be balanced by a set of translational and rotational accelerations, and if we apply the pressure force to represent the weight of battery box, the total mass will be smaller than that in the reality, thus making the acceleration in the simulation larger than in the reality.
The areas where skis support the chassis should be constrained in z-axis (DOF 3) as in lifting case and gravity field should be applied to the whole system. The normal forces from four braking systems are 750 N for each and braking forces are 500 N for each. All of them will be applied on the node where the forces occur in the reality. For example, the friction force in the reality will occur in the area where friction braking
33 pad contacts the I-shape beam and the friction force will be placed on the node in the center of that area.
According to the simulation, the displacement and von-Mises stress of the braking loading case are shown in Figure 22 and Figure 23. The red color implies that the stress there will be over 120 MPa and displacement is over 2 millimeters, which will cause failure. Apparently, there are many red points in these two figures, which is the connection parts between the chassis and two braking systems. The maximum stress in braking case is 200.6 MPa, much higher than 120 MPa.
Thus, the performance of the current chassis design in braking case is bad and must be improved.
Figure 22. Displacement of chassis in lifting case
Figure 23. Stress of chassis in braking case
4.1.3 Acceleration case
Similar to braking case, mass nodes are used to represent all the components and connected to the nodes of the corresponding connection areas by 1D element, RBE3.
34 The areas where people hold the pod should be constrained in z-axis (DOF 3) and gravity field should be applied to the whole system. The acceleration force from one linear induction motor are 3000 N, which will be applied on the node where the forces occur in the reality as in braking case.
One big difference from the braking case is that one extra force will be applied on the ski to balance the weight of the skis. During the process of acceleration, the magnetic levitation system will work and the whole pod will be suspended. At this moment, the skis actually support the whole pod in z-direction, which implies that the total reaction force in the connection area between chassis and skis is equal to the total weight of the pod minus the weight of the skis and magnetic levitation system.
According to the simulation, the displacement and von-Mises stress of the lifting loading case are shown in Figure 24 and 25. The red color implies that the stress there will be over 120 MPa and displacement is over 2 millimeters, which will cause failure.
Apparently, there are many red points in two figures, which is the connection parts between the chassis and two braking systems. The maximum stress in acceleration case is 153.4 MPa, much higher than 120 MPa.
Thus, the performance of the current chassis design in acceleration case is bad and must be improved.
Figure 24. Stress of chassis in braking case
35 Figure 25. Stress of chassis in braking case
4.1 Chassis optimization
Step 1: Increase the thickness
Since the current chassis design will fail in both braking and acceleration processes, optimization cannot be conducted right now. The first step is to make the maximum Von-Mises stress in all loading cases within the safety range. In this sense, the thickness of critical parts where braking systems locate should be increased to increase the stiffness. As shown in Figure 26, the thickness of the purple parts will be increased from 3 mm to 5 mm. The other parts won’t be changed.
Figure 26. Chassis model with different properties
Then the maximum stress in braking and acceleration processes is lower than 120 MPa as shown in Figure 27 and 28, which implies that we can start the optimization analysis to remove some unnecessary material.
The mass increases from 21.5 kg to 28 kg.
36 Figure 27. Stress of chassis in acceleration case
Figure 28. Stress of chassis in braking case
Step 2: Size optimization
Size optimization is used to determine the proper thickness of components to achieve the objective under limitations. In Figure 29, the red and blue color components are designable parts and two beams are non-designable parts. In the optimization analysis, only designable parts will be included.
By setting the objective as minimizing the total mass and the constraint that the displacement of all nodes in y-direction cannot exceed 2 millimeters and maximum Von-Mises stress cannot exceed 120 MPa, the thickness of blue parts and red parts are 1.845 mm and 3.832 mm respectively.
The total mass is reduced from 28 kg to 20.1 kg.
37 Figure 29. Size optimization result of chassis
Step 3: Topology optimization
The constraints and objective of topology optimization is the same as size optimization analysis. The element density is a scale to assess how different parts contribute to the whole stiffness. For parts with higher value of element density, they contribute more to the stiffness. In Figure 30, the parts in the center of the chassis are most blue, implying that some parts can be removed without influencing the whole stiffness a lot.
Figure 30. Topology optimization result of chassis
According to the topology result, the chassis is redesigned and the new design is shown in Figure 31. Compared with the original design, some holes and squares are made on the chassis and some components with low element density are removed. After that, the mass decreases from 20.1 kg to 17.06 kg.
38 Figure 31. Chassis new design
Step 4: Second round of size optimization
In the first round of size optimization, the thickness of the whole designable component will be changed completely. However, there is an alternative way to just increase the thickness of some critical areas in one component while maintaining the thickness of the other areas in same component that one extra sheet aluminum can be welded to the critical area to increase its stiffness.
In this sense, different properties are assigned more detailed to the chassis as shown in Figure 32. Yellow area implies the critical parts that contribute a lot to the whole stiffness.
Figure 32. Chassis with different properties for critical and noncritical parts
39 Final result is listed in Table 4
Table 4. Result of chassis optimization
Optimized Thickness (mm) Manufacturable Thickness (mm)
Gray parts 2.022 2
Blue parts 1.988 2
Orange parts 4.574 4.5
Green parts 2.501 3
Step 5: Reanalyze the new design
After determining the thickness of new chassis design, structural analysis should be done again to ensure that new design fits all requirements.
The results of stress, strain and displacement are shown below. In Figure 33, red color implies that the stress in the chassis is larger than threshold value, 120 MPa.
In Figure 34, red color implies that the strain in the chassis is larger than threshold value, 0.2%. In Figure 35, red parts imply that the displacement in the chassis is larger than threshold value, 2 mm. Since there are no red parts, the new design meets the requirements perfectly.
Figure 33. Stress of chassis in braking case
40 Figure 34. Strain of chassis in braking case
Figure 35. Displacement of chassis in braking case
The mass of chassis decreases from 28 kg to 12.55 kg, reducing 55.2% of the original weight.
4.2 Shell structure analysis
The shell will be fixed on two beams of the chassis. These connection areas should be constrained on all degrees of freedom. There are three loading forces applied on the shell, drag force of the air in the test tunnel, gravity and reaction force from the chassis.
It is quite clear that during the braking process, the stress and strain on the shell will be largest since the directions of drag force and reaction force from the chassis are the same. From aerodynamic group in KTH Hyperloop, the pressure field file is available. By using the “linear interpolation” function, Hypermesh can add pressure to the shell from the data of pressure field file. The reaction force from the chassis is equal to the acceleration times the mass of the shell. We can accomplish easily by adding a gravity field to the shell and defining the field vector along the longitude direction as deceleration value.
With all external forces and constraints defined, structural analysis can be run.
As illustrated before, there are three types of failure theories of composite materials.
41 The results of maximum strain theory, Hsai-Wu failure theory and Hashin failure theory are shown in Figure 36, 37 and 38.
When the composite failure index is less than 1, there won’t exist failure in the structure. To meet the requirement of safety factor as 2, the failure index should be less than 0.5. Since the composite failure index in all three theories are much less than 0.5, we can conclude that the current shell design is awesome.
Figure 36. Failure index of max strain theory in braking process
Figure 37. Failure index of Tsai-WU theory in braking process
42 Figure 38. Failure index of Hashin theory in braking process
4.3 Chassis Optimization with Composite Material
Since carbon fiber is lighter and more rigid than aluminum, there is an alternative method to reduce the weight of chassis by replacing some parts of the chassis with the carbon fiber.
From Figure 33, it’s clear that the central part connected with the linear induction motor is non-critical areas with much lower stress. In this sense, a new model is constructed with carbon fiber. The laminate is built as shown in Figure 39 as [0/45/90/−45]𝑠, which is the same as shell laminate. The only difference is that the zero-direction of fiber is along y-direction.
Figure 39. Laminate of the central part of the chassis
43 Figure 40. Fiber direction of the central part of the chassis
All other settings are the same as what we have done in chassis analysis section.
Since the chassis suffers more external forces during the braking process because of larger deceleration, it is not so necessary to put the failure index results of all loading cases in this report. The composite failure index results of braking procedure are shown below
Figure 41. Failure index of Hashin theory in braking process
44 Figure 41. Failure index of Tsai-Wu theory in braking process
Figure 41. Failure index of Max strain failure theory in braking process
Similarly, the red color implies the failure in the structure as before. Thus, it can be concluded that it’s a good way to use carbon fiber and aluminum together to construct the
The total mass reduces from 12.55 kg to 11.71 kg.
45
5 DISCUSSION AND CONCLUSIONS
A discussion of the results and the conclusions that the author have drawn during the Master of Science thesis are presented in this chapter.
5.1 Discussion
At the beginning, the optimization of the shell part is within the scope, which will contain free size optimization, size optimization and shuffle optimization. However, the optimization result of free size optimization doesn’t show anything. Insteadly, Hypermesh just decreases the thickness of all plies to the minimum manufacturable thickness, which is defined in the manufacturing constraints. When the applied pressure field is increased by ten times, the result is normal. The possible reason might be that the pressure that acts on the shell is too low that the software doesn’t consider it is necessary to remove some material.
It would be the best to redo the CFD analysis of the shell and apply the pressure field to the shell in Hypermesh. Even though it is possible to use carbon fiber to build the whole or part of the chassis, there will exist a lot of extra work to redesign the mounting method and component interfaces since the volume and mounting way are totally different for composite material from aluminum.
For the new design of the chassis, sheet aluminum will be welded to the component to increase some critical areas’ stiffness without increasing the thickness of the whole component. However, the property of a weld part is a bit different from a unit part, which should be studied in the future.
5.2 Conclusions
In this thesis project, structure analysis is conducted for both shell and chassis. With the analysis results, the performance of the current can be concluded. Moreover, the critical areas are figured out so that the improvement ideas are made.
The performance of chassis is not good. There will exist failure in both acceleration and braking processes. Thus, the thickness of some parts must be increased to fit the requirement of safety factor.
An iterative process is taken during the optimization process of the chassis to try to decrease the total weight of the chassis. The total weight of chassis decreases from 28 kg to 11.71 kg, which is a huge improvement.
For shell part, due to the low internal pressure in the test channel, the drag force applied on the shell is really small so that the current design is rigid enough. The optimization process should be conducted in the future.
46
47
6 RECOMMENDATIONS AND FUTURE WORK
In this chapter, recommendations on more detailed solutions and/or future work in this field are presented.
6.1 Recommendations
The material of chassis is aluminum because of its flexibility of manufacturing and high tolerance of fault. In this thesis project, the weight of chassis is reduced by removing unnecessary material and replacing some aluminum parts of the chassis by carbon fiber.
However, there is another way to reduce the weight dramatically by using the carbon fiber to construct the whole chassis.
The difficulty is that the mounting parts of carbon fiber components are totally different from those of aluminum components and the thickness will be much thicker than aluminum, which implies that many components must be redesigned completely.
Nevertheless, for other students continue working on this thesis project, chassis made of carbon fiber is a possible better solution to the problem.
6.2 Future work
Due to the limitation of time and effort, there are a lot of aspects of this thesis project that can be improved in the future as shown below:
● Redo CFD analysis of the shell part and import the data to the structural analysis to increase the accuracy of the final results
● Spot weld connection parts should be included in the simulation of the chassis part
● Redo shell optimization part to figure out whether it is possible to decrease the weight more
● Chassis made of carbon fiber might be a possible solution to decrease the weight as much as possible
48
49
7 REFERENCES
1. Musk, Elon (August 12, 2013). "Hyperloop Alpha" (PDF). SpaceX.
Retrieved August 13, 2013.
2. Gonzalez, Oscar (22 July 2019). "Elon Musk plans trickier Hyperloop test tunnel after speed record broken". Retrieved 23 July 2019.
3. Daryl L. Logan (2011). A first course in the finite element method. Cengage Learning. ISBN 978-0495668251.
4. http://www.recoilengineering.com/finite-element-analysis. Retrieved 25 June 2016.
5. Haertel, Jan Hendrik Klaas (2018). Design of Thermal Systems Using Topology Optimization.
6. Elhajjar, Rani; La Saponara, Valeria; Muliana, Anastasia, eds. (2017). Smart Composites: Mechanics and Design (Composite Materials). CRC Press.
7. https://www.researchgate.net/figure/Various-types-of-fiber-reinforced-composite- lamina_fig1_308721666. Rertieved Sep 2016.
8. http://www.aerospacengineering.net/strength-criteria-of-composite-material- supported-by-fem-analysis/. Retrieved June 2017.
9.https://www.engineering.com/DesignSoftware/DesignSoftwareArticles/ArticleID/1 0938/How-to-Predict-Composite-Failure-Using-Simulation.aspx. Retrieved Sep 2015.
10. Nachiketa Tiwari. Introduction to Composite Materials and Structures. Indian Institute of Technology Kanpur
11. SpcaeX (2018). SpaceX Hyperloop Test Track and Pod Specifications 12. KTH Hyperloop (2019). Final Design Report for SpaceX.
13. Jian Xiong, Liu Ma (2010). Fabrication and crushing behavior of low density carbon fiber composite structures.
14. https://www.alibaba.com/product-detail/Carbon-Fiber-Honeycomb- Panel_60785768160.html. Retrieved 2010
15. https://aerospaceengineeringblog.com/sandwich-panel/. Retrieved June 2013.
50
51
APPENDIX A: GANTT CHART
52
APPENDIX B: RISK ANALYSIS
Risk Impact Probability Solutions
Program not running successfully
Deliverable not complete
Moderate Keep in contact with supervisor and ask for help Boundary conditions
not proper
Deliverable not good Moderate Discuss more with professors and supervisors
Not enough time Deliverable not complete
Low Update Gantt chart and push myself
