\documentclass[12pt]{article}

\usepackage{answers}
\usepackage{setspace}
\usepackage{graphicx}
\usepackage{enumitem}
\usepackage{multicol}
\usepackage{mathrsfs}
\usepackage{geometry}
\usepackage{amsmath}%
\usepackage{amsfonts}%
\usepackage{amssymb}
\geometry{
	a4paper,
	total={170mm,257mm},
	left=15mm,
	right=15mm,
	top=20mm,
}
\usepackage{amsmath,amsthm,amssymb}
\usepackage{graphicx}
\graphicspath{ {D:/} }
\usepackage[english]{babel}
\usepackage[utf8]{inputenc}
\usepackage{fancyhdr}
\usepackage{subcaption}
\usepackage{float}
\usepackage[export]{adjustbox}

\usepackage{caption}
\captionsetup[figure]{font=scriptsize}
% You can choose whatever you want
% scriptsize
% footnotesize
% small
% normalsize
% large
% Large
 
\newcommand{\N}{\mathbb{N}}
\newcommand{\Z}{\mathbb{Z}}
\newcommand{\C}{\mathbb{C}}
\newcommand{\R}{\mathbb{R}}

\DeclareMathOperator{\sech}{sech}
\DeclareMathOperator{\csch}{csch}
 
\newenvironment{theorem}[2][Theorem]{\begin{trivlist}
\item[\hskip \labelsep {\bfseries #1}\hskip \labelsep {\bfseries #2.}]}{\end{trivlist}}
\newenvironment{definition}[2][Definition]{\begin{trivlist}
\item[\hskip \labelsep {\bfseries #1}\hskip \labelsep {\bfseries #2.}]}{\end{trivlist}}
\newenvironment{proposition}[2][Proposition]{\begin{trivlist}
\item[\hskip \labelsep {\bfseries #1}\hskip \labelsep {\bfseries #2.}]}{\end{trivlist}}
\newenvironment{lemma}[2][Lemma]{\begin{trivlist}
\item[\hskip \labelsep {\bfseries #1}\hskip \labelsep {\bfseries #2.}]}{\end{trivlist}}
\newenvironment{exercise}[2][Exercise]{\begin{trivlist}
\item[\hskip \labelsep {\bfseries #1}\hskip \labelsep {\bfseries #2.}]}{\end{trivlist}}
\newenvironment{solution}[2][Solution]{\begin{trivlist}
\item[\hskip \labelsep {\bfseries #1}]}{\end{trivlist}}
\newenvironment{problem}[2][Problem]{\begin{trivlist}
\item[\hskip \labelsep {\bfseries #1}\hskip \labelsep {\bfseries #2.}]}{\end{trivlist}}
\newenvironment{question}[2][Question]{\begin{trivlist}
\item[\hskip \labelsep {\bfseries #1}\hskip \labelsep {\bfseries #2.}]}{\end{trivlist}}
\newenvironment{corollary}[2][Corollary]{\begin{trivlist}
\item[\hskip \labelsep {\bfseries #1}\hskip \labelsep {\bfseries #2.}]}{\end{trivlist}}
 
 \pagestyle{fancy}
 \fancyhf{}
 \rhead{CMT}
 \lhead{Bazan - Call - Cattoni  }
 \rfoot{Page \thepage}
 
 
\begin{document}

% --------------------------------------------------------------
%                         Start here/ Heading
% --------------------------------------------------------------

\title{Computational Mechanics Tools}%replace with the appropriate homework number
\author{Assignment 1 - Fem Modelling: Introduction\\ %if necessary, replace with your course title
Cattoni Correa Domingo Eugenio} %replace with your name
\date{}
\tableofcontents
\pagebreak
\listoffigures
\pagebreak
\listoftables
\pagebreak
%\maketitle
%--------------------------------------------------------------------------
%                               Body
%--------------------------------------------------------------------------

\section{Introduction}
Nowadays, track bed structures need to be elastic to minimise the forces applied to supports as trains pass over them. In rail tracks where no ballast is added, highly elastic elastomer components are placed between the rail and the sleeper (or baseplate) to absorb such loads. However, on ballast beds, these rail pads (elastomeric mats) are also used to reduce high-frequency vibrations. These vibrations are channelled into the ballast bed throughout the rails, thus preventing the ballast form being shattered\cite{southamptonwebsite}.\\

Modern rail fastening systems with such elastomeric mats allow rails to countersink while using the load-transferring effect in rails and dispersing any vertical forces that arise. Notwithstanding that, these components also provide insulation against more than possible vibrations and structure-borne sound produced by any kind of irregularities in the wheels or in the same track. This way, they ensure these vibrations are not transmitted into the ground or just to a minimum extent and thus have little effect on secondary air-borne sound in the adjacent buildings.\\

Other incomes of noise and vibration of concern to railways apart from the aforementioned noise generated at discontinuities or due to severe features in the track or wheel (crossings, rail joints, welds or wheel flats) are the listed below \cite{Calenberg Ingenieure}.\\

\begin{itemize}
	\item Squealing as wheels traverse curves of tight radius.
	\item Wheel-rail rolling noise. Noise caused by vibrations of the wheel and rail which are excited at their contact by irregularities of the running surfaces.
	\item Low frequency ground-borne vibration occurred in locations where soil is soft. There, vibration propagates parallel to the ground surface with a low rate of attenuation with distance. These kinds of vibrations concern for heavy freight operations.
	\item Noise from trains in tunnels (ground-borne noise). It happens to occur as vibration of the track is transmitted through the ground and radiated as sound within the tunnel building by vibration of their walls.
	\item Engine noise.
	\item Above 300 km/h, aerodynamic noise from trains is to be significant.
	\item Noise radiated from bridges. Vibration of the track is transmitted into the bridge structure, which in turn radiates low frequency sound. 
\end{itemize}

The present study assesses the efficiency of some elastomeric mats designs through the analysis of their stiffness.

\section{Problem state}
The problem statement is given in such a way some of data is already obtained experimentally.\\

Considering the following:

\begin{itemize}
	\item Test mat sample placed between two rigid plates that applies the stress uniformly.
	\item Area: 300 x 300 $mm^2$.
	\item Commuter line subjected to a total load resulting from:
	\begin{itemize}
		\item Static load: dead weight of the track superstructure: $\sigma_{0}=2N/mm^2$
		\item Dynamic load from the train passage: $\sigma_{d}=1N/mm^2$
	\end{itemize}	
	\item $\gamma = 1.4$ is the amplification factor (for a train speed of 80 km/h)
	\item F= 5 Hz of excitation frequency.
\end{itemize}

The study is carried out by means of different points.
Firstly, it is calculated analytically the static stiffness of a massive mat considering only the static case. The features of this mat are:

\begin{itemize}
	\item Young modulus = 1.3 GPa
	\item Poisson’s coefficient = 0
	\item H = 25mm.	
	\item Density = 800 $kg/m^3$
\end{itemize}

A metallic plate, where the force is applied with the following considerations:

\begin{itemize}
	\item Young modulus = 210 GPa
	\item Poisson’s coefficient = 0.3
	\item H = 25mm.	
	\item Density = 7800 $kg/m^3$
\end{itemize}

To model the contact in between the mat and the plate, different constraints are taken into account.\\

Afterwards, the model is generated by means of FEM (using Abaqus) in order to proof the results obtained above.\\   

Secondly, two designs are proposed with the aim of optimising material efficiency. By taking as a reference the first case, these two new proposals are compared in terms of stiffness efficiency. These design can be seen in the following subsection.

Thirdly, an analysis of the dynamic response of the massive mat is performed.
And finally, an improvement of the two previous design is made so as to analyse the issues to be cleared in these proposals.\\
 
Moreover, some considerations are taken when performing the analysis.
To point out some aspects, when referring to the units it is to clarify that International System is adopted. However, millimetre instead of meter is used when using length as physical measurement.\\

For the geometry, two solids are designed. One for the steel plate and the other for the elastomeric mat with the properties highlighted before. 

%------------------------------------Begin Methodology--------------------------------------
\section{Methodology}
In this section it will be discussed and explained several calculation methodologies used in this work, such as volume determination, types of contact used or how dynamic loads were applied in the model among others. 

\subsection{Volume determination}
In order to compare new designs of the elastomeric mat, where the aim is optimize material efficiency (i.e. achieve same stiffness with less material) and then check which one is the most efficient in terms of stiffness/volume, the volume of each design was needed to compute, taking into account the volume of the massive elastomeric mat as a reference.\\ 
In figure below can be seen the massive elastomeric mat and three new design to be analysed, taking into account the volume condition (all geometries have to have the same volume). 
	
\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=50mm]{Q1_masive_plate}
	\includegraphics[width=50mm]{Q2_DA}
	\includegraphics[width=50mm]{Q2_DB}\\
	\centering
	\caption {Desgin to be analysed. Left: Massive mat. Centre: Design A. Right: Design B} 
	\label{fig:1}
\end{figure}

In figure \ref{fig:2} can be observed, for each design, several section dimensions. For design A and B can also be seen the dimension, which name is H2, has not value. In order to determine H2, all volume must be the same and thus be able to satisfy the volume condition.

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=100mm]{Q1_a}
	\includegraphics[width=100mm]{Q2_b}
	\includegraphics[width=100mm]{Q2_a}\\
	\centering
	\caption {Dimensions. Top: Massive mat. Centre: Design A. Bottom: Design B. All expressed in mm.} 
	\label{fig:2}
\end{figure}

An important remark, the depth value for all models, including the massive mat, will be equal to 300 mm and will be called H3 (H3 = 300 mm for all models). 

\begin{enumerate}
	\item Massive mal volume $(M_{vol})$ = $H*L*H_3 = 2250000 mm^3$.
	\item Design A volume $(DA_{vol})$ = $H_3*(H_2*L+5*H_1*(b+a)) = 300*(300*H_2+1500) $
	\item Design B volume $(DB_{vol})$ = $H_3*(H_2*L-5*H_1*a) = 300*(300*H_2-1500) $
\end{enumerate}

Once computed each volume, all of them must be equal, and equation to be solved is:

\[M_{vol} = DA_{vol} \longrightarrow H_{2A} = 20 mm\]
\[M_{vol} = DB_{vol} \longrightarrow H_{2B} = 30 mm\]

Finally, for design A and B, $H_2$ was called adding a subscript A and B in order to differentiate to which model correspond.\\ 

\captionsetup{belowskip=1pt,aboveskip=1pt}
\begin{table}[H]
	\caption{Final dimensions.}
	\label{tab:T1}
	\begin{center}
\begin{tabular}{|c|c|c|c|c|c|c|c|}
	\hline 
	Design & a [mm] & b [mm] & c [mm] & H1 [mm] & H2 [mm] & H3 [mm] & L [mm] \\ 
	\hline 
	Massive & -- & -- & -- & -- & 25 & 300 & 300 \\ 
	\hline 
	Design A & 10 & 20 & 10 & 10 & 20 & 300 & 300 \\ 
	\hline 
	Design B & 20 & 20 & -- & 15 & 30 & 300 & 300 \\ 
	\hline 
\end{tabular} 
\end{center}
\end{table}

\subsection{Contact and interface models}

In order to model the interface between the elastomeric mat and the steel plate, three kind of contact model was taken into account. The first model was called "coincident nodes" and was used in order to compare the stiffness obtained by hand and by analysis. The second model was a surface-to-surface contact model, where friction effects and no penetration conditions were considered, and the last one was tied constrain model, where mat and steel contact surfaces will be stick one each other. 

\begin{enumerate}
\item \textbf{Coincident nodes model}

The idea of this model was to take mesh nodes of the interface and make them coincident. In figure below can be appreciated the model said before.   

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=150mm]{Cnodes}\\
	\centering
	\caption {Coincident nodes model.} 
	\label{fig:3}
\end{figure}

In order to perform this model, the mat and steel plate were meshed similarly, and then being able to merge nodes.\\
Usually, this sort of interface models are performed in order to avoid setting up contact in models, due to contact models are very expensive from the computational point of view. In general coincident mesh nodes models are widely used to model rigid or permanent joints such as weld or glue joints among others. Sometime, to simplify the simulation, this kind of models work well taking some precautions. This is the case of the model used to compute the first part of the present work.    

\item \textbf{Surf-to surf contact model}

This kind of models are used to obtain more realistic results. In this context, friction effect and no penetration conditions are been in mind.  

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=150mm]{Csurf}\\
	\centering
	\caption {Coincident nodes model.} 
	\label{fig:4}
\end{figure}

In figure below can be appreciated that different meshes have been used for the elastomeric mat and steel plate. The reason why these two meshes are dissimilar follow the fact that when the master and slave regions have different mesh densities, more elements on the slave region will mean that more contact elements are created, which will produce a more accurate solution.

It's important to understand how contact element are created when selecting which region will be the master and which the slave, since the two can be interchangeable. The solver projects vector normals from the master region to the slave region. It then creates contact elements when these normals intersect elements in the slave region and are within the search distance criteria for the contact pair. This means that when the two regions of a pair do not have corresponding one-to-one elements, the number of contact elements that the solver creates can change depending on which region it projects the elements from and which region it projects them to \cite{contact}, \cite{abaqus}. In figure \ref{fig:5} can be observed a theoretical explanation of why is important to select master-slave region carefully.

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=80mm]{master-slave}\\
	\centering
	\caption {Theoretical explanation of contact behaviour.} 
	\label{fig:5}
\end{figure}

\item \textbf{Tie constraint}

fully constrained contact behaviour is defined using tie constraints. A tie constraint ties two separate surfaces together so that there is no relative motion between them. This type of constraint allows to fuse together two regions even though the meshes created on the surfaces of the regions may be dissimilar.

Surface-based constraint using a master-slave formulation and the constraint prevents slave nodes from separating or sliding relative to the master surface. In figure below can be seen the generated tie constraint model \cite{abaqus}.

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=100mm]{tie}\\
	\vspace{0.5cm}
	\includegraphics[width=100mm]{tie1}\\
	\centering
	\caption {Tie constraint. Top: Master and slave meshes. Bottom: generated tie constraint painted in black.} 
	\label{fig:6}
\end{figure}
\end{enumerate}


\subsection{Dinamic load}

In order to analyse the dynamic response of the mat, a dynamic load was applied. The mathematician expression of it load is:

\[\sigma(t) = \sigma_0+\sigma_d*\gamma*\sin(\omega*t)\] 

Where: $\omega = 2*\pi*f$ and $\sigma_0$ is the static load.\\

Figure below shows the plot of the dynamic load used in the model.

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=80mm]{dload}\\
	\vspace{0.2cm}
	\centering
	\caption {Dynamic load.} 
	\label{fig:7}
\end{figure}

To analyse the dynamic response of the mat, Abaqus/CAE software was used. This software has the capability of introducing several sort of load, in particular dynamic loads as the loading shown before.\\ 
In order to introduce this kind of load, two steps were followed. First, was needed to define the harmonic amplitude, and then the dynamic load as a pressure load.\\

Figure \ref{fig:8}, first step. Definition of amplitude.

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=100mm]{amp}\\
	\vspace{0.2cm}
	\centering
	\caption {First step: Amplitude definition.} 
	\label{fig:8}
\end{figure}

Figure \ref{fig:9}, second step. Definition of pressure load or uniform distribute load.

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=80mm]{load}\\
	\vspace{0.2cm}
	\centering
	\caption {Second step: Uniform load definition.} 
	\label{fig:9}
\end{figure}

\subsection{Performed analysis}

In order to compute the mat stiffness and the dynamic response, two analysis types were considered. First, to compute the mat stiffness a static linear analysis was performed and then, to compute the dynamic response a dynamic implicit analysis was carried out. Non-linear effects were not considered.   

For the dynamic response, small time increments were taken into account for an accurate representation of the displacement-time graphic. It can be observed in figure below.

\begin{figure}[H]
\centering
\captionsetup{justification=centering}
\includegraphics[width=60mm]{dset}\\
\vspace{0.2cm}
\centering
\caption {Dynamic response analysis. Set up.} 
\label{fig:10}
\end{figure}

%------------------------------------End Methodology----------------------------------------

%-------------------------------Begin Results and Discussionss-------------------------
\section{Results and Discussions}
In this section, the obtained results will be shown and discussed for each model and analysis performed.\\
Results and models will be correlated in order to make sure that the obtained one has physical meaning. In addition, a by hand calculation will be added in order to compare it with obtained result by FEM. Also, this section will be split according to the model and analysis type.\\

The following list of model and analysis will show up in the present section:
\begin{enumerate}
	\item Massive mat model and linear static analysis:
	\begin{itemize}
		\item By hand calculation of stiffness.
		\item Coincident nodes mesh model of massive mat and steel plate.
		\item Surf-to-surf contact model of massive mat and steel plate.
		\item Tied constraint model of massive mat and steel plate.
	\end{itemize}
	\item Design A, B and C model and linear static analysis:
	\begin{itemize}
		\item Surf-to-surf contact was used in order to model the interaction between solids.
	\end{itemize}
	\item Massive mat model and dynamic response
\end{enumerate}


\subsection{Results of massive mat model and linear static analysis}
As was mentioned before, the efficiency of these mat is assessed by their stiffness, defined as the stress applied divided by the resulting displacement ($KN/mm^3$). 

\begin{itemize}
\item \textbf{Stiffness obtained by hand:}
	
The mat stiffness was computed, considering elasticity theory and infinitesimal strains.
\[\underline{\underline{\sigma}} = \underline{\underline{\epsilon}}:       	\underline{\underline{\underline{\underline{C}}}}\] 
	
Since Poisson effect are not taken into account and only Y displacement is necessary to compute the stiffness, therefore, a simple 1D linear elastic equation will be used:	
\[\sigma_{yy} = E\cdot\epsilon_{yy}\]	
\[\frac{\sigma_{yy}}{E} = \epsilon_{yy}\]

and $\epsilon_{yy} = \dfrac{dv}{dy}$ $\rightarrow$ $\int_{0}^{h}\frac{\sigma_{yy}}{E}dy$

\[\int_{0}^{h}\frac{\sigma_{yy}}{E}dy = \int_{0}^{h}\frac{\sigma_{0}}{E}dy = \frac{\sigma_{0}}{E}h\]
	
Where: $\sigma_0 = 2\cdot10^{-2} N/mm^2$ (static load) and $E=1300 MPa$

\[v = \frac{2\cdot10^{-2}}{1300}\cdot25mm = 3.85\cdot10^{-4}mm\]

And the stiffness is:

\[S_{hand} = \sigma_{0}/v = \frac{2\cdot10^{-2}}{3.85\cdot10^{-4}\cdot1000} KN/mm^3 = 0.052 KN/mm^3\]\\


\item \textbf{Stiffness obtained by analysis: Coincident nodes mesh model}

Figure \ref{fig:11} shows the vertical displacement. The obtained results were in concordance with the applied load, and the maximum value was equal to $ v = -3.89\cdot10^{-4}$ mm.

\[S_{model1} = \sigma_{0}/v = \frac{2\cdot10^{-2}}{3.89\cdot10^{-4}\cdot1000} KN/mm^3 = 0.051 KN/mm^3\]\\

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=80mm]{Q1_res}\\
	\centering
	\vspace{0.2cm}
	\caption {Coincident nodes mesh model: Vertical displacement $[mm]$.} 
	\label{fig:11}
\end{figure}

As it expected, the result obtained by analysis was equal thus the one obtained by hand. Since the interface or the interaction between plates was modelled using a coincident nodes mesh, all the ingoing energy, was transmitted to the elastomeric mat whitout any loss of it, In addition, the steel plate can be considered as a rigid body, if the Young's modulus of both materials are compared one each other. These two argument explain why these results are almost similar. 

\item \textbf{Stiffness obtained by analysis: Surf-to-surf contact model}

In the following figure can be seen the vertical displacement on the left, and the contact pressure un the right.

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=75mm]{Q1_res_contact}
	\hspace{0.1cm}
	\includegraphics[width=75mm]{Q1_pres_contact}\\
	\vspace{0.2cm}
	\centering
	\caption {Surf-to-surf contact model. Left: Vertical displacement $[mm]$. Right: Contact pressure $[MPa]$.} 
	\label{fig:12}
\end{figure}

From the obtained result can be said some remark. First, the magnitude and direction of the result obtained in this section were in accordance with the applied load. Second, it was observed an uniformed contact pressure, with a maximum value equal to the applied load. This max value was located on the interface between plates. It is means that the contact algorithm worked properly.\\
Finally, it was observed that the model was less stiff than the one shown previously, obtaining a maximum vertical displacement equal to $ v = -4.32\cdot10^{-4}$ mm. This remark can be associated to the fact that the contact model was modelled (Steel plate can move freely in X and Z direction due to Poisson effect and friction effect would not have relevance.)     

\[S_{model2} = \sigma_{0}/v = \frac{2\cdot10^{-2}}{4.32\cdot10^{-4}\cdot1000} KN/mm^3 = 0.046 KN/mm^3\]\\

\item \textbf{Stiffness obtained by analysis: Tied constraint model}

The results related with the last model of this type of mat can be observed in the following figure, where vertical displacement result can be seen.

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=80mm]{Q1_res_tie}\\
	\centering
	\vspace{0.2cm}
	\caption {Tied constraint model: Vertical displacement $[mm]$.} 
	\label{fig:13}
\end{figure}

The maximum vertical displacement was equal to $v = -4.15\cdot10^{-4}$ mm, slightly less than the previous model (surf-to-surf contact model), but greater than the first model shown at the beginning (Coincident nodes mesh model).

\[S_{model3} = \sigma_{0}/v = \frac{2\cdot10^{-2}}{4.15\cdot10^{-4}\cdot1000} KN/mm^3 = 0.048 KN/mm^3\]\\

In descending order, the coincident nodes mesh model was the most stiff one, then, the tied constraint model was the next, and finally, the less stiff model but more realistic was the surf-to-surf model. However, in term of elastomeric mat stiffness, all models were similar, having stiffness values from 0.046 to 0.052 $KN/mm^{3}$.

\subsection{Design A and B result and linear static analysis}

In figure below can be seen the obtained vertical displacement for the two design proposed  before. 

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=75mm]{Q2_desA}
	\hspace{0.1cm}
	\includegraphics[width=75mm]{Q2_desB}\\
	\vspace{0.2cm}
	\centering
	\caption {Design A and B results. Left: Vertical displ. of design A $[mm]$. Right: Vertical displ. of design B $[mm]$.} 
	\label{fig:14}
\end{figure}

It was obtained a maximum vertical displacement for design A equal to $v = -1.095\cdot10^{-3}$ mm, while for design B was equal to $v = -1.033^{-3}$ mm. Both obtained results was similar. 

Instead of computing the volumetric stiffness, since both volumes are equal, the stiffness of each one was calculated, giving the following values.\\

\textbf{Design A Stiffness:}
\[S_{D\textunderscore A} = \sigma_{0}/v = \frac{2\cdot10^{-2}}{1.095\cdot10^{-3}\cdot1000} KN/mm^3 = 0.018 KN/mm^3\]

\textbf{Design B Stiffness:}
\[S_{D\textunderscore B} = \sigma_{0}/v = \frac{2\cdot10^{-2}}{1.033\cdot10^{-3}\cdot1000} KN/mm^3 = 0.019 KN/mm^3\]

In term of stiffness, all designs gave similar results. So, it can be concluded that both model will have similar mechanical behaviour.  

\subsection{Design C}

In this section it is going to be studied another way of designing the original solid mat and the designs presented A and B. To do so, we have taken into consideration the following design that we are going to call C, which is very similar to the design B, since the only difference with it is the division of the squared holes into triangles. The reason behind this that the triangles perform much better in compression if placed in this way, we are going to see how the displacement and stresses are once the load is applied on the structure.

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=80mm]{geometry}\\
	\centering
	\vspace{0.2cm}
	\caption {Improved Design} 
	\label{fig:15}
\end{figure}

In the figure right below, we can see the dimension values taken into consideration in order to include the same volume values as the previous designs.

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=100mm]{sketch}\\
	\centering
	\caption {Sketch of the new design used} 
	\label{fig:16}
\end{figure}

As it has seen, the design proposed has the same volume of material as the designs A and B with the goal ok making a fair comparison between them.\\
Once the geometry of the new proposed mat was drawn, it was time for the computation of static load. Some difficulties appeared in this part of the work since the largest mesh available in the student version software was not enough for the sharp edges and complex geometry displayed above. For this reason, a commercial version of Abaqus was used in order to obtain results. In the figure right below it can be observed how the proposed matt deformed under the vertical loading and the stresses associated to it.

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=90mm]{disp}\\
	\centering
	\vspace{0.2cm}
	\caption {Vertical Displacements  $[mm]$} 
	\label{fig:17}
\end{figure}

Once computed the maximum vertical displacement, the stiffness of this design will be calculated in the same way as previous designs. The following expression is showing the stiffness values of design C.

\textbf{Design C Stiffness:}
\[S_{D\textunderscore C} = \sigma_{0}/v = \frac{2\cdot10^{-2}}{1.269\cdot10^{-3}\cdot1000} KN/mm^3 = 0.016 KN/mm^3\]

As we can see the figures above show the vertical displacements and stresses on the proposed and improved mat. The results show a reduced displacement in the vertical direction, as well as more resistance since the material along the volume had a less unified distribution.\\
In conclusion, it has to be said that the proposed mat will react better under the loads specified by the problem statement, however, it will also be more complicated to manufacture, since the hole geometry is more complex. In addition to this, the geometry was also an inconvenience for the numerical computation. A commercial version of the software was used in order to outcome this problem which had solution using the 1000 node student version.

\subsection{Dynamic response results of massive mat}

Since was mentioned in previous sections, the massive mat was analysed by dynamic response. This sort of analysis was carried out due to the fact that this type of materials and geometries are usually undergone to a dynamic load, similar to the one presented before.

In figure below can be observed vertical displacement vs time for a given central mesh node. As it expected, the plot conserves the harmonic shape.

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=70mm]{Q3_disp}\\
	\centering
	\vspace{0.2cm}
	\caption {Dynamic response: Vertical displacement $[mm]$ at function of time.} 
	\label{fig:18}
\end{figure}

In the next figure can be seen different result at significant times. For instance, points 2 and 3 are pointing the maximum and minimum vertical displacement on the harmonic response. And point 1 is highlighting a dash line that corresponds to vertical displacements, where each value was equal to the one obtained by applying a static stress $\sigma_0$. Therefore, the results are consistency with the static case.

\begin{figure}[H]
	\centering
	\captionsetup{justification=centering}
	\includegraphics[width=70mm]{Q3_disp1}\\
	\includegraphics[width=70mm]{Q3_1}
	\includegraphics[width=70mm]{Q3_2}
	\includegraphics[width=70mm]{Q3_3}\\
	\centering
	\vspace{0.2cm}
	\caption {Dynamic response: Vertical displacement $[mm]$ at different times.} 
	\label{fig:19}
\end{figure}

Finally, it can observed in the vertical displacement (figure \ref{fig:14} or \ref{fig:15}) that theoretically speaking at time t = 0, the static stress should be applied, obtained results similar to the static one. However, at time t = 0 the static load can not be applied instantaneously, and the vertical displacement decreases abruptly with some oscillation. This phenomena would be associated to the fact that the solver has to make some iteration until certain stability is reached. In order to avoid these spurious results, a refinement in terms of time can be performed or enlarge the total time. 
\newpage

\end{itemize}

\newpage
\section{Conclusion}
As a conclusion we can say that the mat design has been studied in different ways such as static and dynamic loads as well as using different designs in order to see how the shape of the elastomeric volume can affect. We have finally determined, that best performance when it comes to static load is the design C.\\
We have also seen is that the Abaqus Student Version has a node limitation of 1000, this was a problem in the development of the project since most of the models created and meshed automatically exceeded by far this number. The solution in this case was the reduction of elements in the longitudinal direction. By doing so, we avoided the reduction of elements in the thickness direction which was the one that had more importance in order to see results.\\
Another issue we find necessary commenting is the isotropic or orthotropic characteristic of the elastomeric material. In the work done, we took into consideration an isotropic material and it should be done in future work a further study of this particularity  to find other results.\\
Finally, it has to be said that the elastomeric mat is one of the key features when it comes to reducing the vibration noise in the railway. However, there are other ways of reducing the vibration of it like the concrete used in the construction, the sleepers placed are a bunch of possibilities that can make a greater difference in this aspect.\\












%---------------------------------------------------------------------------------------------
% End document


\begin{thebibliography}{9}
	\bibitem{contact} 
	Adrian Jansen. 
	\textit{Linear contact analysis: demystified }. 
    White peper, Predictive engineering 2010.
    
    \bibitem{abaqus} 
    \textit{Abaqus/CAE 6.13 User's Manual. }. 
    Dessault Systems 2013
	
	\bibitem{southamptonwebsite} 
	southampton: railway noise and vibration engineering university of southampton 2018
	\\\texttt{https://www.southampton.ac.uk/engineering/research/groups/dynamics/}
	
	\bibitem{Calenberg Ingenieure}
	Calenberg Ingenieure: Elastomeric bearings - Anti-vibration bearings for building construction and track construction - Noise protection.
	\\\texttt{http://www.calenberg-ingenieure.com}
\end{thebibliography}







\pagebreak

\end{document}
