\documentclass[11pt,a4]{article}
\usepackage{fullpage}
\usepackage{setspace}
\usepackage{parskip}
\usepackage{titlesec}
\usepackage[section]{placeins}
\usepackage{xcolor}
\usepackage{breakcites}
\usepackage{lineno}
\usepackage{hyphenat}
\PassOptionsToPackage{hyphens}{url}
\usepackage[colorlinks = true,
linkcolor = blue,
urlcolor = blue,
citecolor = blue,
anchorcolor = blue]{hyperref}
\usepackage{etoolbox}
\makeatletter
\patchcmd\@combinedblfloats{\box\@outputbox}{\unvbox\@outputbox}{}{%
\errmessage{\noexpand\@combinedblfloats could not be patched}%
}%
\makeatother
\usepackage[round]{natbib}
\let\cite\citep
\renewenvironment{abstract}
{{\bfseries\noindent{\abstractname}\par\nobreak}\footnotesize}
{\bigskip}
\titlespacing{\section}{0pt}{*3}{*1}
\titlespacing{\subsection}{0pt}{*2}{*0.5}
\titlespacing{\subsubsection}{0pt}{*1.5}{0pt}
\usepackage{graphicx}
\usepackage[space]{grffile}
\usepackage{latexsym}
\usepackage{textcomp}
\usepackage{longtable}
\usepackage{tabulary}
\usepackage{booktabs,array,multirow}
\usepackage{amsfonts,amsmath,amssymb}
\providecommand\citet{\cite}
\providecommand\citep{\cite}
\providecommand\citealt{\cite}
% You can conditionalize code for latexml or normal latex using this.
\newif\iflatexml\latexmlfalse
\providecommand{\tightlist}{\setlength{\itemsep}{0pt}\setlength{\parskip}{0pt}}%
\AtBeginDocument{\DeclareGraphicsExtensions{.pdf,.PDF,.eps,.EPS,.png,.PNG,.tif,.TIF,.jpg,.JPG,.jpeg,.JPEG}}
\usepackage[utf8]{inputenc}
\usepackage[ngerman,english]{babel}
\usepackage{float}
% Use this header.tex file for:
% 1. frontmatter/preamble LaTeX definitions
% - Example: \usepackage{xspace}
% 2. global macros available in all document blocks
% - Example: \def\example{This is an example macro.}
%
% You should ONLY add such definitions in this header.tex space,
% and treat the main article content as the body/mainmatter of your document
% Preamble-only macros such as \documentclass and \usepackage are
% NOT allowed in the main document, and definitions will be local to the current block.
\newcommand{\beginsupplement}{%
\setcounter{table}{0}
\renewcommand{\thetable}{A\arabic{table}}%
\setcounter{figure}{0}
\renewcommand{\thefigure}{A\arabic{figure}}%
}
\begin{document}
\title{}
\vspace{-1em}
\date{}
\begingroup
\let\center\flushleft
\let\endcenter\endflushleft
\maketitle
\endgroup
\onehalfspacing
\sloppy
\begin{center}
\Huge
\textbf{Numerical Flow Simulation}
\vspace{2.5cm}
\LARGE
\textbf{P2:Collaboration}\\
Report
\vspace{2.5cm}
\Large
Authors: Alex Felice, Nina Gottschling, Benjamin Rahm, Gauvain Ramseier, Nathan Pellaux\\
Instructor: Mark L. Sawley
\vfill
\end{center}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/EPFL-Logo/EPFL-Logo}
\end{center}
\end{figure}
\begin{center}
\vspace{0.8cm}
\Large
EPFL\\
Fall semester 2017
\end{center}
\newpage
\section*{Table of Contents}
\newline
1. Introduction \newline
2. Theoretical Backgroud\newline
2.1 Drag Coefficient\newline
2.2 Lift Coefficient\newline
2.3 Pressure coefficient\newline
2.4 Behaviour of flow depending on angle of attack\newline
2.5 Behaviour of the lift and drag depending on angle of attack\newline
3. Theoretical study\newline
3.1 Application\newline
4. Numerical Analysis\newline
4.1 Choice of an appropriate model and type of mesh\newline
4.2 Domain size\newline
4.3 Methods used in ANSYS Fluent\newline
5. Results\newline
5.1 Results of the Theoretical Simulation\newline
5.2 Results of the Numerical Simulation\newline
5.3 Results of the Experiments\newline
6. Comparison of Results and Conclusion\newline
6.1 Lift coefficient\newline
6.2 Drag coefficient\newline
6.3 Pressure coefficient\newline
7. Appendix\newline
\newline
8. References
\newpage
\section*{Introduction}
The task of this mini-project is to conduct a validation and verification study using a NACA 4-series airfoil. The simple, two dimensional definition of this airfoil makes the application of experimental, theoretical and numerical simulation methods more accessible in the context of a mini-project.\newline
For this validation and verification study there are three main methods in evaluating the slightly cambered NACA 2412 airfoil (Fig. \ref{923445}).
Firstly, there is the experimental study of the airfoil in a wind tunnel at Hepia (HES-SO). Secondly, there is the theoretical study of the airfoil using XFOIL, an interactive program for the design and analysis of subsonic isolated airfoils. Thirdly, the numerical simulation and study of the airfoil will be conducted with a RANS approach using solver such as ANSYS Fluent.
In each part, the relevant aerodynamic quantities such as pressure, lift and drag coefficient are determined, as well as the velocity field around the airfoil.\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/NACA2412-(1)/NACA2412-(1)}
\caption{{NACA 2412 airfoil.\protect\cite{241216.01.2015}
{\label{923445}}%
}}
\end{center}
\end{figure}
\section*{Theoretical Backgroud}
\newline
In all of the three methods used in this project, important aerodynamic properties of an airfoil, which is a cut parallel to xy-plane of a wing, will be evaluated.
For the experiment in the wind tunnel a constant cord wing spanned over the whole width of the tunnel is used, hence, the air flow sees a so-called "infinite wing". As the airfoil has the same geometry as the wing in the xy-plane, the properties along the wing and the airfoil are the same. If one wants to obtain data for an actual wing, there are some problems as the properties of a finite wing differ, and so such measurements are only an approximation.
\subsection*{Drag Coefficient}
With the drag coefficient the complex dependencies of shape, inclination, and flow conditions on aircraft drag can be modeled. The drag coefficient $C_{d}$ is equal to the force along the x-axis divided by half the density, $\rho$, times the velocity $V_{\infty}$ squared times the airfoil chord $c$.
\begin{equation}
C_{d} = \frac{F_{x}}{\frac{1}{2}\rho V_{\infty}^2 c}
\end{equation}
In order to make this quantity more accessible one can define quantity one half of the density times the velocity squared, which is called the dynamic pressure $q$. So
\begin{equation}
C_{d} = \frac{F_{x}}{qc}
\end{equation}
Then, the drag coefficient expresses the ratio of the drag force to the force to the dynamic pressure times airfoil chord.\cite{coefficient}
\subsection*{Lift Coefficient}
For an airfoil,
the lift coefficient is used to model the complex dependencies of shape, inclination, and some flow conditions on lift. The lift coefficient $C_{l}$ is equal to the force along the y-axis divided by half the density times the velocity squared times the airfoil chord $c$.
\begin{equation}
C_{l} = \frac{F_{y}}{\frac{1}{2}\rho V_{\infty}^2c }
\end{equation}
With $q$, the dynamic pressure:
\begin{equation}
C_l = \frac{L}{q A}
\end{equation}
Then, the lift coefficient expresses the ratio of the lifting force to the force produced by the dynamic pressure times the airfoil chord $c$.\cite{coefficienta}
\subsection*{Pressure coefficient}
The pressure distribution over an airfoil is not uniform and vary especially with the angle of attack. For this reason is convenient to work with a nondimensional coefficient just like for the lift and the drag. Thus we can introduce the pressure coefficient $C_p$ as:
\begin{equation}
C_p=\dfrac{p-p_{\infty}}{\frac{1}{2}\rho V_{\infty}^2}
\end{equation}
where $p$ is the static pressure at the point of interest and $ p_{\infty}$ is the static pressure of the free stream flow (i.e. far from any disturbance).\cite{2013}
\subsection*{Behaviour of flow depending on angle of attack}
In our simulations, the flow is always considered at steady state. According to the theory of aerodynamics the boundary layer on the upper surface of the airfoil is laminar for small angles of attack, so there is no boundary layer transition on the upper surface. Indeed, there is no transition between laminar and turbulent flow on the airfoil. An increase of the angle of attack will create a transition near the trailing edge of the foil, but the attached flow is still dominant. An even larger increase of the angle will move this separation layer closer to the leading edge. At a certain angle of attack, the separation layer will quickly move upstream resulting in a mostly turbulent flow on the upper surface and a drop in the lift of the foil. This angle is the critical angle of attack where the stalling occurs. The range of the critical angle is between 8\selectlanguage{ngerman}° and 20° for classical wings. (cc.\cite{anderson2017}, pg. 46ff)
\subsection*{Behaviour of the lift and drag depending on angle of attack}
For a wing at a given shape, the lift coefficient, $C_{l}$, and the drag coefficient, $C_{d}$, only depend on the angle of attack (Fig. \ref{771786}).
$C_{l}$ increases linearly until the stalling point after which it sharply decreases. This can be explained by the mean of the pressure distribution over the airfoil: the reduced pressure on the upper surface, due to the increase of the velocity around the airfoil, is tending to push the section upward while the one on the lower surface tends to push the section downward. Normally for an airfoil the effect on the upper surface is larger and the resultant force that push upward the section is the lift (Fig. \ref{257817}).
$C_{d}$ has a minimum value at a small angle of attack and increases with the angle of attack. The shape of the graph of the drag coefficient depending on the angle of attack is parabolic. A large negative angle of attack also has a higher drag coefficient. The minimum velocity before stalling at a certain altitude and for a certain plane is therefore defined by $C_{l}$, there are multiple solutions to artificially increasing the maximum lift, however these methods are not addressed in this report. On the other hand the maximum velocity is determined by the minimal drag coefficient. Therefore, there are two important angles of attack that must be determined. These are the angle where $C_{l}$ is maximal, the critical point, and the angle at which $C_{d}$ is minimal, it gives us the minimally necessary thrust and, therefore, is a possibility for fuel savings. Finally, we are interested in the relation between the lift and drag coefficients depending on the angle of attack (Fig.\ref{479992}) to find the best ratio. Classical lift to drag ratio is between 15 and 20 for a plane cruising, which means for an angle of attack of 0°.
Further, it can be mentioned that the faster an airplane flies, the lower the required value of $C_{l}$ is.(cc.\cite{anderson2017}, pg. 46ff)\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.56\columnwidth]{figures/Cl-and-Cd-versus-alpha-(theorie)/Cl-and-Cd-versus-alpha-(theorie)}
\caption{{Lift and drag coefficient in function of the angle of
attack.\protect\cite{anderson2017}
{\label{771786}}%
}}
\end{center}
\end{figure}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/Cp/Cp}
\caption{{Typical pressure distribution around an airfoil
{\label{257817}}%
}}
\end{center}
\end{figure}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/L-D-ratio-VS-angle-of-attack/L-D-ratio-VS-angle-of-attack}
\caption{{Lift to drag ratio as a function of the angle of
attack.\protect\cite{anderson2017}
{\label{479992}}%
}}
\end{center}
\end{figure}
\section*{Theoretical study}
XFOIL \cite{Drela_1989} is a code that uses a panel method, as well known as aerodynamic potential flow code, to predict aerodynamic properties of a 2D flow around an airfoil. It was developed by Mark Drela at MIT. The panel method is combined with a boundary layer analysis to take into account viscous effects near the airfoil. A particularity of XFOIL is that it is possible to perform an inverse design with this code. Nowadays, XFOIL and other panel codes are used predominantly for preliminary aerodynamic analysis as they are time efficient. For more accurate results, CFD software such as Fluent is required.
A panel code can be used to estimate the fluid velocity and pressure distribution around a wing for instance. XFOIL uses a linear-vorticity stream function formulation, that was chosen such that it allows inverse design and the incorporation of a boundary layer analysis to the panel code. The airfoil shape and the wake trajectory are divided into flat panels. These flat panels have a linear vorticity distribution, only for the airfoil panels, and a constant source strength - this term "links" the inviscid flow to the viscous boundary layer. The stream function is required to be equal to a constant at the extremities, i.e. nodes, of each panel and this requirement allows to obtain a linear system. This system can be solved directly for inviscid flows, but needs other equations for viscous flows as described below.
A limitation of these panel codes is that it is valid for inviscid flows only. Thus, the viscous effects which are not negligible near the airfoil are not taken into account by the panel code. To remedy this problem, the XFOIL code uses a fully-coupled viscous/inviscid interaction method. The code accounting for the viscous effect is mainly based on the ISES code, a transonic analysis code also developed by Drela \cite{DRELA_1987}. It uses a two-equation lagged dissipation integral BL formulation and an envelope $e^n$, with $n_{crit} = 9$ as the default value, transition criteria. The wall transpiration concept is used to model the interaction between the boundary layer and the inviscid flow. This is achieved by relating the source strength term mentioned earlier to the gradient of the mass defect.
As previously mentioned, it is possible to perform two types of analysis with XFOIL: direct and inverse. The direct one is the common one, where we define a geometry and look for a pressure distribution. The other one is, as its name indicates, the inverse procedure, where we define a speed distribution and look for a geometry. This method is referred as full-inverse. There is actually a third type of analysis, called mixed-inverse procedure. It is a mix of the two above procedures, where we first run a simulation with the direct method on an airfoil to obtain a speed distribution and then run an inverse procedure with this speed distribution but allowing only certain parts of the airfoil to be modified.
\subsection*{Application}
In order to obtain the desired result using XFoil there are few steps to do. Firstly, we will have to load the desired airfoil into XFoil using the command: "XFOIL c$>$ NACA 2412". Secondly, in order to start the calculation we have to enter the OPER sub-level: "XFOIL c$>$ OPER". This will produce the prompt ".OPERi c$>$", where the "i" means that XFoil is operating in the inviscid mode. By typing "visc" in the prompt, Xfoil switches to the viscous mode. We are then asked to introduce a Reynolds number:
\begin{equation}
Re=\dfrac{\rho V_{\infty}c}{\mu}
\end{equation}
It is important to remember that XFoil works with a unity chord length, $ c=1 $, so we have to put the corresponding Reynolds number. Before running the calculations for the desired series of angles of attack we need to increase the number of iterations to at least $500$ in order to achieve converge for the biggest angles of attack. Then, the command ".OPERv c$>$ pacc" will create a file in which the section lift, drag and momentum coefficient along with upper and lower transition points will be saved. Once the file is created and named, we can proceed with the calculations by using the command: "aseq -4 20 2", which will execute Xfoil for a series of angles of attack, from -4 to 20 degrees with a step of 2 degrees.
\section*{Numerical Analysis}
\newline
\subsection*{Choice of an appropriate model and type of mesh}
First, we will introduce the quantity $y^+$; it describes how coarse or fine the mesh is. $y^+$ depends on the friction viscosity, the density of the fluid, the distance between the wall and the nearest node.
\begin{equation}
y^+ = \dfrac{\rho u y }{\mu}
\end{equation}
\newline
with
\newline
$ \rho =$ density of the fluid
\newline
$ u = $ friction velocity
\newline
$ y = $ distance from the wall to the nearest node
\newline
$ \mu $ = dynamic viscosity
\newline
We know the free stream velocity, the density, the dynamic velocity and the boundary layer and the wall distance. We can compute the friction velocity, $u$, from the wall shear stress; the formula of the wall shear stress is:
\begin{equation}
\tau_w = C_f \cdot \frac{1}{2} \, \rho \, U_{freestream}^2
\end{equation}
it gives us $ u = \sqrt{\frac{\tau_w}{\rho}} $.
For the numerical analysis a Reynolds-average approach (RANS), where the turbulence is averaged to model all scale lengths. In the solver ANSYS fluent for each angle of attack two turbulence models were used. Firstly, the one equation Spalart Allmaras model and, secondly, the two equation, realizable $k-\epsilon$ model, were used. The realizable $k-\omega$ model was used as well, but it showed poor convergence or divergence at some angles of attack and, therefore, we do not include it in the further analysis. (Fig. \ref{366702})
The Spalart Allmaras turbulence model works well for airfoil flow simulations. It works well in situations when the flow is not detached and wall bounded, as in the present case, and, when, boundary layers are subjected to adverse pressure gradients. The weakness of Spalart Allmaras is based on the fact that it needs a fine mesh at the boundary, $y^+ = 1$, and that it is not accurate enough for high Reynolds numbers.
The SST $k-\omega$ model, which stands for shear stress tensor $k-\omega$ model, has proven its quality in numerous applications such as for wind turbines and for situations with boundary layers with adverse pressure. It uses two different equations, depending where we are in the model. The SST $k-\omega$ uses the $k-\omega$ model in the inner parts of the boundary layer and in the free stream. It requires a rather small mesh resolution near the wall, $y^+< 10$.
In our case, the mesh has a size of $12 mm$ at the wall and a finer mesh of $0.5 mm$ at the wall of airfoil. The $y^+$ was computed at the wall and at the foil. (see Appendix, Fig. \ref{942569} and \ref{305400})
As an example, for the mesh with a angle of attack of 16\selectlanguage{ngerman}°, we have a $y^+$ varying from less than one to $30$ around the airfoil which is small, but not sufficient for using the Spalart Allmaras method. As mentioned before, the Spalart Allmaras method needs a $y^+$ of $1$ or smaller in order to deliver accurate results. It is worse for an angle of attack of 0° as $y^+$ varies from $5$ to almost $40$ at the airfoil profile.
$y^+$ varies from $300$ to $400$ at the wall which is huge but not important as we are not interested in the flow at the wall.
The mesh used is a triangle mesh on the domains where a precise computation is not needed, such as the wall or the inlet. It is a coarse mesh. Where the mesh needs to be fine, a Cmesh is used. In this type of mesh rectangle meshes at the foil profile and at the trailing edge are used. Using triangles at the profile would not be a wise choice, because reducing the height of the mesh will only flatten the triangle. In our case, there is a rectangular mesh close to the foil. A Cmesh is good in order to compute the wake, but relies on the assumption that the areas where the wake is are known approximately. Here, there is always the risk that the wake is not where the mesh was refined.
\subsection*{Domain size}
The domain reaches from the inlet to the outlet. A velocity at the inlet and the pressure at the outlet were fixed. The size of the domain will impact the results as follows:
if one chooses an inlet too close to the leading edge of the airfoil, the velocity of the free stream will be influenced by the airfoil and, therefore, wrong. On the other hand, the further we fix the inlet, the bigger the domain is. It means more computation time for each simulation. The trade-off lies at a distance of two or three times the chord of the foil.
The choice of the outlet is motivated by the same reason as the choice of the inlet, except that the interfering parameter is the wake produced by the foil. A reasonable choice is to have at least, the outlet fixed at a distance of five times the chord of the foil.
In our case, the inlet is fixed at a distance of two times the chord which is the minimum, if the $V_{inlet}$ should undergo few influences from the foil. There is a distance of five times the chord from the trailing edge to the outlet, which is also the minimum. It could explain the non optimal results that we get. As the recommended distance from the inlet to the leading edge is between two and three times the chord and the distance between the trailing edge and the outlet should be at least five times the chord length.
\subsection*{Methods used in ANSYS Fluent}
\newline
Further, a time steady, pressure-based solver was used, as there is no interdependance between density, energy, momentum and other quantities and the flow is not dependent on time and is at steady state. Pressure based solvers were originally developed for low-speed flows and the pressure is determined from the pressure or pressure-correction equation, which are obtained from the continuity and momentum equations. Also the velocity was formulated with its absolute value. In order to compare the numerical results with the experimental results, an inflow velocity of $36.5 \frac{m}{s}$ was used. This velocity is the average of the velocities appearing in the experiments; they ranged from $34.5 \frac{m}{s}$ to $39.6 \frac{m}{s}$. The fluid was assumed to be air and have a constant density and viscosity, as set in the reference values (Fig. \ref{976284}).\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.42\columnwidth]{figures/ansysref/paramfluent}
\caption{{Reference values as set in Fluent for all models.
{\label{976284}}%
}}
\end{center}
\end{figure}
For the solution methods the coupled scheme was used, as this usually converges faster. In combination with the pressure-based solver, the coupled scheme is usually used for incompressible flows with low velocities, as in the case for the analysis of the NACA 2412 airfoil in a wind tunnel which is attacked at different angles with a flow velocity of $36.5 \frac{m}{s}$.
For the spatial discretization the second-order upwind scheme was used for all available quantities, i.e. the pressure, momentum and modified turbulent viscosity. As it leads more accurate results than the first-order scheme. However, it is slower and less robust, which was not a problem in our analysis. Here the face values are obtained through multi-dimensional reconstruction.
For the gradient of the spatial discretization the Green-Gauss node-based method was used. Here the Green-Gauss theorem, that relates the gradient at the cell center to weighted average of values at the cell face, is used. In the node-based Gauss-Green method the cell-face values are calculated by arithmetically averaging the values at all nodes. We used this method as it is more accurate for unstructured meshes.\newline
\section*{Results}
\newline
\subsection*{Results of the Theoretical Simulation}
The general trend that we observe in usual cases (Fig. \ref{771786}) appears at least qualitatively for both the lift and drag coefficient as a function of the angle of attack.
There might be some discrepancies for the larger angles of attack. As mentioned before, for angles between 8\selectlanguage{ngerman}° and 20°, stalling occurs for general wings. The XFOIL user guide \cite{guide} reports that near stall, the accuracy of prediction tends to decrease. We precisely notice this decrease in accuracy, as for these angles the results of our methods differ. This loss of accuracy is partly due to the approximation made in the viscous formulation when an angle is specified. XFOIL first estimates the wake trajectory from an inviscid solution at the desired angle and then uses it to get the viscous solution. In reality, the viscous effect modify the wake trajectory and XFOIL does not account for that. It has a negligible effect at small angles of attack but it is not the case near or past stall. The values of velocity, density and viscosity used to calculate the Reynolds number in XFoil are the same showed in Fig. \ref{976284}.
\subsection*{Results of the Numerical Simulation}
As mentioned earlier, three different models were used - the Spalart Allmaras, realizable $k-\epsilon$ and SST $k-\omega$ model. The $k-\omega$ model was the least convincing method, as it showed weak convergence without overly adjustment of the relaxation factors in the Fluent parameters. Therefore, we decided not to run the numerical simulation for all angles with the $k-\omega$ model. It was used for 12°, 16° and 20° (Fig. \ref{366702})
The following diagram, Fig. \ref{697059}, shows the monitored lift coefficient using the SST $k-\omega$ model at an angle of attack of 12°. This serves as an example of a non-converging solution using this method.\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/Notconverging/Notconverging}
\caption{\selectlanguage{ngerman}{The monitoring of the lift coefficient at 12° using the SST k-Omega
model in Fluent.
{\label{697059}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}
Figure \ref{495930} shows the results obtained using the Spalart Almaras and realizable $k-\epsilon$ models in Fluent. It shows that up to an angle of attack of 8° the predictions for $C_d$ and $C_l$ are in very good agreement. After this angle the predictions for $C_l$ differ, which is most likely do to the beginning of stalling and due to the fact, that the Spalart Almaras model is less accurate for turbulent flow.\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/pdfresizer-com-pdf-crop/Comparison-Numerical-1}
\caption{{Lift and drag coefficients obtained in Fluent.
{\label{495930}}%
}}
\end{center}
\end{figure}
\newline
The Spalart Allmaras and realizable $k-\epsilon$ methods showed rather good results. However, we know from the theory that the former model is not a sufficiently good method when the boundary layer detaches. For this reason, we decided to rely on results provided by the realizable $k-\epsilon$ model. The computed $C_{l}$ in both models alligns with the trend predicted by the theory, as there is a linear increase until a critical point and then a sharp drop of the lift coefficient with increasing angle of attack. The $C_{d}$ as predicted by both models is coherent with the theory and does not differ hugely in both models.
The critical point is between an angle of attack of 12\selectlanguage{ngerman}° and 16° for the realizable $k-\epsilon$ model and at around 12° for the Spalart Allmaras method, which are acceptable results. For the solutions obtained by the realizable $k-\epsilon$ model the velocity magnitude and direction at 12° and 20° around the airfoil was visualized using ParaView.(Fig. \ref{148481} and \ref{803324})
In Figure \ref{803324}, it can be seen that at an angle of attack of 20° there is a significant increase of turbulent flow above the airfoil. The length and coloring of the displayed vectors is scaled by the local velocity. While in Figure \ref{148481} it can be seen that in the area above the airfoil at an angle of attack of 12° the flow is still attached, whereas at 20° the separation layer begins at the leading edge of the foil and stalling is obviously taking place.
Further, the solutions obtained converged as the monitored drag and lift coefficients did not change after maximally $800$ iterations; we let the solver run for $1000$ iterations in the most cases. If for a certain angle of attack the chosen model did not converge within $1000$ iterations, we let the solver run for $2000$ iterations, which usually yielded converging results.
Concerning the verification of the models used; as described above the Spalart Almaras and realizable $k-\epsilon$ models yielded the predictions as described by used Fluent tutorials and Fluent user guides. For example, the Spalart Almaras model was said to not produce accurate results in the regime of turbulent flow, which was visible when comparing the results to the experimental results and the ones produced by the $k-\epsilon$ model.(Fig. \ref{495930} and \ref{405798})
Concerning the validation of the implemented models, the $k-\epsilon$ model yielded a better agreement to the experimental data than the Spalart Almaras model. However, at large angles of attack, i.e. above 12°, both models did not yield sufficiently accurate results.\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.91\columnwidth]{figures/12kepsvel/keps12}
\caption{\selectlanguage{ngerman}{Velocity direction around the airfoil at an angle of attack of 12° where
the color indicates the velocity in m/s.
{\label{148481}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.91\columnwidth]{figures/20kepsvel-pdf-pvtmp/keps20}
\caption{\selectlanguage{ngerman}{Velocity direction around the airfoil at an angle of attack of 20° where
the color indicates the velocity in m/s. ~
{\label{803324}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}
\subsection*{Results of the Experiments}
The experiments were conducted in the small subsonic wind tunnel at Hepia in Geneva. It has a test section of $0.305\times0.305 m^2$ and length of $0.6 m$, and a maximum upstream speed of $38.5 \frac{m}{s}$. As the air was not blown into the wind tunnel, but sucked out by a ventilator the inflow speed depended on the angle of attack. This was due to the wing blocking the airflow through the tunnel. Hence, the velocities in the experiment ranged from $34.5 \frac{m}{s}$ to $39.6 \frac{m}{s}$. This might lead to a further difference between the experimental, theoretical and numerical predictions, as the latter two methods used a constant velocity. The temperature, pressure and density were the same as in the reference values set in Fluent, Fig. \ref{976284}. The wing that was used was an extension of the NACA 2412, with the same profile along the width of the tunnel.The obtained results of the lift and drag coefficient are in agreement with the general theoretical predictions as mentioned in the section "Theoretical Background". (See Appendix, Fig. \ref{374740})
\newline
\section*{Comparison of Results and Conclusion}
\newline
\subsection*{Lift coefficient}
As shown in Fig. \ref{405798} and \ref{449822}, the numerical simulation using the realizable $k-\epsilon$ model and the theoretical calculation using XFOIL yield a good prediction for the lift coefficient for small angles of attack. When approaching the critical point the predictions obtained using XFOIL are increasingly less accurate, as explained in previous sections. The results obtained using the $k-\epsilon$ model are of sufficient accuracy up to an angle of attack of 16°, which corresponds to the critical point. The relative error of $3.5\%$ at this point is more than satisfying.\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.63\columnwidth]{figures/Lift-comparison/Lift-Coefficient1}
\caption{{Comparison between the three methods of the lift coefficient in function
of the angle of attack.
{\label{405798}}%
}}
\end{center}
\end{figure}
\newline
After this point the numerical results are wrong. Indeed, the relative error of $C_{l}$ to the experimentally obtained value is of $99.93\%$ at 20\selectlanguage{ngerman}°. The average absolute error of $C_{l}$ with respect to the experimental data, without taking in account the values for 20°, is $ 0.12 $ and the relative error is of $ 28.10\%$. While the average absolute error of the XFoil approach, always without the 20° case, is $ 38.15\% $. We can conclude that although there are some errors in the obtained values, the general trend of the lift coefficient of our results is coherent with the theory and experiment.\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.84\columnwidth]{figures/Relative-error-lift/Relative-Error-Lift-Coefficient}
\caption{{Relative errors on the lift coefficient with respect to the experimental
data
{\label{449822}}%
}}
\end{center}
\end{figure}
\subsection*{Drag coefficient}
As shown in Fig. \ref{655425} and \ref{855057}, the numerical simulation using the realizable $k-\epsilon$ model shows a good prediction of the flow. The theoretical prediction using XFOIL is, like for the lift coefficient, satisfactory only at small angles of attack.
The maximum absolute error with respect to the experiment for the numerical approach is of $\Delta C_{d} = 0.0228$ and the largest relative error is of $39\%$. The average of the absolute error is of $\Delta C_{d} = 0.0088$ and the average of the relative error is of $17.26\%$. Also in this case the results of XFoil give a higher relative error than for the numerical simulation, with an average value of $86.6\%$.\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/Drag-comparison/Drag-Coefficient}
\caption{{Comparison between the three methods for the drag coefficient in
function of the angle of attack.
{\label{655425}}%
}}
\end{center}
\end{figure}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/Relative-error-drag/Relative-Error-Drag-Coefficient}
\caption{{Relative errors on the drag coefficient with respect to the experimental
data ~
{\label{855057}}%
}}
\end{center}
\end{figure}
\subsection*{Pressure coefficient}
Unfortunately we do not have the experimental data in order to calculate the pressure coefficient, so in this section we can just compare the $C_p$ for the numerical simulation and the theoretical one. In XFOIL (Fig. \ref{956252} and \ref{964842}), the pressure coefficient is given along the boundary layer around the airfoil, where the yellow line corresponds to the upper surface and the blue one to the lower surface. The dashed line is the $C_p$ distribution for an inviscid flow. The large negative values of $C_p$ at higher angle of attack are confirmed by the theory \cite{anderson2017} which is indicative of a high local flow speed. At even higher angles of attack the upper surface pressure reduction suddenly collapse near the leading edge, meaning that the little lift remaining is only due to the lower surface pressure increase. We can also see once again that at small angles of attack the two methods gives similar results(Fig.\ref{956252} to \ref{824193}), while when the flow starts to separate (visible thanks to the boundary layers) the Xfoil results strats to diverge from the numerical one (Fig. \ref{532775} to \ref{274671}).\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.63\columnwidth]{figures/Cp-xfoil-0/Cp-xfoil-0}
\caption{\selectlanguage{ngerman}{Cp at an angle of incidence of 0°obtained with XFOIL.
{\label{956252}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.63\columnwidth]{figures/Pressurecoef-0deg-3methods/Cp-0-fluent}
\caption{\selectlanguage{ngerman}{Cp at an angle of incidence of 0°obtained with the numerical method. ~
{\label{305562}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.63\columnwidth]{figures/Cp-xfoil-20/Cp-4-xfoil}
\caption{\selectlanguage{ngerman}{Cp at an angle of incidence of 4° obtained with XFOIL. ~
{\label{964842}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.63\columnwidth]{figures/20degpressurecoef/Cp-4-fluent}
\caption{\selectlanguage{ngerman}{Cp at an angle of incidence of 4° obtained with the numerical method.
{\label{824193}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}
\pagebreak
\section*{Appendix}
\beginsupplement
~\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.63\columnwidth]{figures/wallYplus-alpha0/wallYplus-alpha0}
\caption{\selectlanguage{ngerman}{y+ at an angle of attack of 0° at the airfoil and tunnel.
{\label{942569}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.63\columnwidth]{figures/WallYplus-alpha16/WallYplus-alpha16}
\caption{\selectlanguage{ngerman}{y+ at an angle of attack of 16° at the airfoil and tunnel. ~
{\label{305400}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/data/Data-comparison}
\caption{{Lift and drag coefficients as obtained in all three methods.
{\label{681016}}%
}}
\end{center}
\end{figure}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/ldexp/ldexp}
\caption{{Lift and drag forces obtained in the experiments.
{\label{374740}}%
}}
\end{center}
\end{figure}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=1.00\columnwidth]{figures/Large-Table1/Ansys-Final+Diagramm-xlsx---Tabellenblatt2}
\caption{{Data obtained for different models in Fluent.
{\label{366702}}%
}}
\end{center}
\end{figure}
\pagebreak\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/Cp-8-xfoil/Cp-8-xfoil}
\caption{\selectlanguage{ngerman}{Cp at an angle of incidence of 8° obtained with XFOIL. ~ ~
{\label{532775}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/Cp-8-fluent/Cp-8-fluent}
\caption{\selectlanguage{ngerman}{Cp at an angle of incidence of 8° obtained with the numerical method.
{\label{172773}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/Cp-12-xfoil/Cp-12-xfoil}
\caption{\selectlanguage{ngerman}{Cp at an angle of incidence of 12° obtained with XFOIL. ~ ~
{\label{165549}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/Cp-12-fluent/Cp-12-fluent}
\caption{\selectlanguage{ngerman}{Cp at an angle of incidence of 12° obtained with the numerical method. ~
{\label{428675}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/Cp-16-xfoil/Cp-16-xfoil}
\caption{\selectlanguage{ngerman}{Cp at an angle of incidence of 16° obtained with XFOIL. ~ ~
{\label{202348}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}\selectlanguage{english}
\begin{figure}[H]
\begin{center}
\includegraphics[width=0.70\columnwidth]{figures/Cp-16-fluent/Cp-16-fluent}
\caption{\selectlanguage{ngerman}{Cp at an angle of incidence of 16° obtained with the numerical method. ~
{\label{274671}}%
}}
\end{center}
\end{figure}\selectlanguage{ngerman}
\selectlanguage{english}
\FloatBarrier
\bibliographystyle{plainnat}
\bibliography{bibliography/converted_to_latex.bib%
}
\end{document}