Rans Simulation of Supesonic Jets

UNIVERSIDAD POLITÉCNICA DE MADRID
ESCUELA TÉCNICA SUPERIOR DE INGENIERÍA
AERONÁUTICA Y DEL ESPACIO
GRADO EN INGENIERÍA AEROESPACIAL
TRABAJO FIN DE GRADO
RANS Simulation of Supersonic Jets
AUTOR: Adrián ÁLAMO SANZ
ESPECIALIDAD: Propulsión Aeroespacial
TUTOR PROFESIONAL: Daniel RODRÍGUEZ ÁLVAREZ
TUTOR ACADÉMICO: Fco Javier DE VICENTE BUENDÍA
Febrero de 2020

Resumen
Hoy en d´ıa, el ruido proveniente de los aviones es un aspecto importante.
Tanto si vives cerca de un aeropuerto o una base militar, o quieres una cab-
ina de avión más silenciosa y billetes más baratos, el ruido juega un papel
crucial. A largo plazo, el objetivo de este TFG es ser el primero en abrir
un camino a la investigación sobre este problema. Asimismo, su objetivo
principal, más allá del contenido, es servir como gu´ıa a futuros estudiantes
para iniciarse en este problema, y ser parte de un proyecto más grande.
Este TFG tiene como meta, en cuanto a contenido, el cálculo del flujo
medio turbulento a la salida de una tobera convergente en condiciones de sal-
ida supersónicas. La geometr´ıa de la tobera y condiciones del flujo provienen
de un experimento realizado por la Universidad de Poitiers, Francia. Los re-
sultados finales serán comparados con aquellos del experimento de Poitiers.
Primeramente, extraeremos la geometr´ıa de la tobera CAD proporcionada
por la Universidad de Poitiers. El experimento llevado a cabo en esta Uni-
versidad sirve como referencia. Sin embargo, es emp´ırico, y los resultados
son obtenidos directamente de un flujo real, y no una simulación numérica,
como el nuestro.
En segundo lugar, el proceso de mallado y exportación de la malla al
código CFD. Los distintos software utilizados son mostrados. La serie de
pasos presentados, necesarios para llegar de la geometr´ıa CAD, pasando por
los diferentes software, hasta llegar a la malla deseada que dar al solver.
En tercer lugar, las simulaciones numéricas hechas usando el código TAU−
Flow. Los distintos parámetros numéricos de la simulación CFD son definidos.
Finalmente, el post-procesado de los datos y caracterización del flujo
medio, incluyendo la longitud del núcleo potencial, definición de la región
anular de la capa de mezcla y formación de patrones de ondas de choque.
ii

Abstract
Nowadays, noise coming from aircraft is an important issue. Whether you
live close to an airport or a military base, or you simply want a quieter air-
craft cabin and cheaper tickets, noise plays a crucial role. On the long term,
the goal of this thesis is to be the first one to open a research path on this
issue. Furthermore, its main goal, apart from its content, is to serve as a
guide for future students to initiate on this problem, and be part of the big-
ger project.
This thesis has, as its main objective content-wise, the computation of
the mean turbulent flux at the exit of a convergent nozzle in supersonic con-
ditions. The nozzle geometry and flow conditions come from the experiment
carried out by the Université de Poitiers, France. The final results, will be
compared with those of the Poitiers experiment.
Firstly, we will be extracting the geometry from the CAD nozzle provided
by the Université de Poitiers. The experiment carried out in this University
serves as a reference. However, it is empirical, and results obtained directly
from an actual jet, and not a numerical simulation, like ours.
Secondly, the meshing process and exportation of the mesh to the CFD
code. The various software used are shown. A series of steps are presented in
order to get from the CAD geometry, through the different software, switch-
ing formats, until a desired mesh to feed the solver is reached.
In third place, the numerical simulations run using the TAU −Flow code.
The different numerical parameters of the CFD simulation are defined.
Finally, the postprocessing of the data and characterization of the mean
flux, including the length of the potential core, definition of the anular mixing
layer region and formation of shock wave patterns.
iv

A mam´a y pap´a, sin los que nada de esto hubiese sido posible.
A mi hermano, siempre referente.
vi

Contents
List of Figures ix
List of Tables xiii
List of Symbols xvii
List of Acronyms xix
1 Introduction 1
1.1 Supersonic Jets and Nozzles . . . . . . . . . . . . . . . . . . . 1
1.1.1 Modes of Operation . . . . . . . . . . . . . . . . . . . . 3
1.2 Description of the Exhaust Jet in a C and CD Nozzle . . . . . 7
1.2.1 Structure of the Jet . . . . . . . . . . . . . . . . . . . . 8
1.2.2 Shock Diamonds and Mach Disks . . . . . . . . . . . . 9
1.3 CFD-TAU . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15
1.3.1 Computational Fluid Dynamics Overview . . . . . . . 15
1.3.2 The DLR TAU-Code R
. . . . . . . . . . . . . . . . . . 18
1.4 Objectives and Structure of this Thesis . . . . . . . . . . . . . 22
2 Pre-processing: from CAD Geometry to Mesh 25
2.1 Scheme of the Process . . . . . . . . . . . . . . . . . . . . . . 25
2.2 Extraction of the Geometry of the Nozzle . . . . . . . . . . . . 26
2.3 Generation of the 2D Meshes . . . . . . . . . . . . . . . . . . 32
2.4 Export to a TAU Format Mesh . . . . . . . . . . . . . . . . . 37
3 Solver: Numerical Simulations Set-Up 41
3.1 Deﬁnition of the Flow Parameters . . . . . . . . . . . . . . . . 41
3.2 Boundary Conditions . . . . . . . . . . . . . . . . . . . . . . . 42
3.3 Turbulence Model . . . . . . . . . . . . . . . . . . . . . . . . . 43
3.4 Numerical Parameters . . . . . . . . . . . . . . . . . . . . . . 46
viii

4 Post-processing: Results 49
4.1 Description of the Results . . . . . . . . . . . . . . . . . . . . 49
4.2 Mesh Convergence Test . . . . . . . . . . . . . . . . . . . . . . 57
4.3 Simulations with and without Nozzle Geometry . . . . . . . . 60
4.4 Mean Flux Characterization . . . . . . . . . . . . . . . . . . . 64
5 Overview and Conclusions 66
Bibliography 69
ix

List of Figures
1.1 Scheme of a CD Nozzle. . . . . . . . . . . . . . . . . . . . . . 2
1.2 Behaviour of a CD Nozzle depending on the exit pressure with
respect to the ambient pressure. . . . . . . . . . . . . . . . . . 4
1.3 Modes of operation of a CD Nozzle as a function of the pres-
sure ratio p/p0. [4] . . . . . . . . . . . . . . . . . . . . . . . . 6
1.4 Modes of operation of a CD Nozzle as a function of the Mach
number M. [4] . . . . . . . . . . . . . . . . . . . . . . . . . . . 6
1.5 Schematic representation of the structure of an under-expanded
jet. [6] . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9
1.6 Petals or ”Turkey feathers” of a variable area nozzle in a Eu-
rofighter Typhoon EF2000. . . . . . . . . . . . . . . . . . . . . 10
1.7 Nozzle of the Aerojet Rocketdyne RS-25, also known as the
Space Shuttle main engine (SSME). . . . . . . . . . . . . . . . 10
1.8 XRS-2200 linear Aerospike Engine Nozzle for the X-33 program. 11
1.9 Wave structures that create shock diamonds in an under-expanded
flow. [3] . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12
1.10 Wave structures that create shock diamonds in an over-expanded
flow. [3] . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12
1.11 Mach diamonds structure in the J58 engine of the SR-71 ”Black-
bird” running with afterburner. . . . . . . . . . . . . . . . . . 13
1.12 Mach diamonds structure in a F-15 Eagle. . . . . . . . . . . . 13
1.13 Mach diamonds structure in a F-16 Falcon. . . . . . . . . . . . 13
1.14 Summary of the phenomena at the trailing edge of a nozzle in
function of the exit pressure. . . . . . . . . . . . . . . . . . . . 14
1.15 The three main elements of a CFD analysis. [13] . . . . . . . 17
1.16 Example of a structured mesh. [13] . . . . . . . . . . . . . . . 17
1.17 Example of an ustructured mesh. [13] . . . . . . . . . . . . . . 18
1.18 Representation of the finite volume method for a structured
and unstructured grid. [13] . . . . . . . . . . . . . . . . . . . . 19
1.19 Example of multiple domains of TAU parallel grid partition-
ing. [11] . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19
x

1.20 Example of the TAU preprocessor dual grid approach. [11] . . 20
1.21 Example of the TAU preprocessor number of multigrid levels.
[11] . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20
1.22 Example of TAU grid adaptation. Local grid refinement. [11] . 21
1.23 Example of TAU grid deformation. Deflection of the tip of a
wing of an aircraft. [11] . . . . . . . . . . . . . . . . . . . . . . 21
2.1 Views from different perspectives of the C nozzle used in this
thesis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 27
2.2 Contour of the C nozzle used, extracted in SpaceClaim. . . . . 27
2.3 Measurements of the C nozzle expressed in millimeters. . . . . 28
2.4 General measurements of the Fluid Domain. . . . . . . . . . . 29
2.5 Fluid Domain for a Structured Mesh. . . . . . . . . . . . . . . 30
2.6 Detailed view of the nozzle geometry region of the structured
domain. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 30
2.7 Fluid Domain for an Unstructured Mesh. . . . . . . . . . . . . 31
2.8 Detailed view of the nozzle geometry region of the unstruc-
tured domain. . . . . . . . . . . . . . . . . . . . . . . . . . . . 31
2.9 Geometry of fluid domain without nozzle. . . . . . . . . . . . 32
2.10 Detailed view of the region of the domain without nozzle. . . . 32
2.11 Structured mesh with nozzle geometry. . . . . . . . . . . . . . 33
2.12 Structured mesh with nozzle geometry. Detailed view. . . . . . 33
2.13 Structured mesh with nozzle geometry. Detailed view. . . . . . 34
2.14 Unstructured mesh with nozzle geometry. . . . . . . . . . . . . 34
2.15 Unstructured mesh with nozzle geometry. Detailed view. . . . 34
2.16 Example of a 3D extruded mesh. . . . . . . . . . . . . . . . . 35
2.17 Example of the markers used for the mesh with nozzle geometry. 36
2.18 Example of the markers used for the mesh without nozzle ge-
ometry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 37
2.19 Module icem2tau in Bender. . . . . . . . . . . . . . . . . . . 38
2.20 Module setup taugrid in Bender. Step 1 of the process. . . . 38
4.1 Mach number as a function of the reference diameter, for the
Poitiers experiment. . . . . . . . . . . . . . . . . . . . . . . . 50
4.2 x velocity profile as a function of the reference diameter, for
the Poitiers experiment. . . . . . . . . . . . . . . . . . . . . . 51
4.3 Evolution over time of the supersonic jet. Starting at 10000
iterations (top right), until 50000 iterations (bottom right). . . 52
xi

4.4 Colour scheme of the pressure field of our solution for 50000
iterations. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 53
4.5 Mesh without nozzle geometry, showing the influence on our
solution. It is focused on the potential core region, where more
refinement is applied. . . . . . . . . . . . . . . . . . . . . . . 53
4.6 Evolution of the Mach Number over time for the mesh without
nozzle geometry. . . . . . . . . . . . . . . . . . . . . . . . . . . 56
4.7 Evolution of the pressure over time for the mesh without nozzle
geometry. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 56
4.8 Evolution of the velocity on the x axis over time for the mesh
without nozzle geometry. . . . . . . . . . . . . . . . . . . . . . 57
4.9 Evolution of the residuals over time. Meshes with and without
the nozzle geometry, and structured and unstructured, first
refinement. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 58
4.10 Unstructured mesh, with the potential core region extended
and refined, in a rectangular region. . . . . . . . . . . . . . . . 59
4.11 Unstructured mesh, with an extended cone-shaped region re-
fined. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 60
4.12 Evolution of the Mach number with nozzle geometry, for a
structured and unstructured mesh, and different degrees of
refinement. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 60
4.13 Evolution of the Mach number without nozzle geometry, for
a structured and unstructured mesh, and different degrees of
refinement. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 61
4.14 Evolution of the Mach number with and without nozzle ge-
ometry, for a structured and unstructured mesh, and different
degrees of refinement. . . . . . . . . . . . . . . . . . . . . . . . 61
4.15 Example of the structured mesh without nozzle geometry. . . . 62
4.16 Example of the results obtained for the mesh with nozzle ge-
ometry. Top left: first refinement structured mesh. Top right:
second refinement structured mesh. Bottom left: first refine-
ment unstructured mesh. Bottom right: second refinement
unstructured mesh. . . . . . . . . . . . . . . . . . . . . . . . . 62
4.17 Example of the results obtained for the mesh without nozzle
geometry. Top left: first refinement structured mesh. Top
right: second refinement structured mesh. Bottom left: first
refinement unstructured mesh. Bottom right: second refine-
ment unstructured mesh. . . . . . . . . . . . . . . . . . . . . . 62
4.18 Example of the results of the unstructured mesh with noz-
zle geometry. Colour scheme of the Mach number for 50000
iterations. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 63
xii

4.19 Evolution of the Mach number over time, for the unstructured
mesh with nozzle geometry. . . . . . . . . . . . . . . . . . . . 63
xiii

List of Tables
4.1 Number of elements for the first refinement meshes. . . . . . . 58
4.2 Number of elements for the second refinement meshes. . . . . 58
xv

List of Symbols
x Position
A Area
u Velocity
M Mach number
p Total pressure
ρ Total density
T Total temperature
Q Mass flow rate
h Total enthalpy
R Ideal gas constant
cp Specific heat capacity at constant pressure
cv Specific heat capacity at constant volume
γ Adiabatic index
c Local sound velocity
D Reference Diameter
Re Reynolds number
Pr Prandtl number
µ Sutherland reference viscosity
Subscript
0 Stagnation (total) property
∞ Free-stream quantity
e Exit of the nozzle properties
t Throat cross-section
1, 2 Different positions along the Nozzle
∗ Sonic flow / Critical state property
j Fully-expanded jet conditions
xvii

List of Acronyms
C Convergent
CD Convergent-Divergent
CFD Computational Fluid Dynamics
RANS Reynolds-Averaged Navier-Stokes
URANS Unsteady Reynolds-Averaged Navier-Stokes
CAD Computer Aided Design
LUSGS Lower-Upper Symmetric Gauss-Seidel
CFL number Courant–Friedrichs–Lewy number
NPR Nozzle Pressure Ratio
xix

Chapter 1
Introduction
1.1 Supersonic Jets and Nozzles
Supersonic jets have many technological applications, and are used for dif-
ferent industrial purposes. Within the aeronautics industry, we encounter
internal (engines) and external (aerodynamic) flows.
Furthermore, in the rocket business, supersonic jets are applied in missiles
and rocket boosters. For instance, a familiar situation in which supersonic
conditions can be reached, is at cruise conditions of the jet of civilian aircraft.
Mach number may vary between 0.8 up to 1.2.
A crucial part in the design of a supersonic engine is its nozzle. ”A nozzle
(from nose, meaning ’small spout’) is a tube of varying cross-sectional area
(usually axisymmetric) aiming at increasing the speed of an outflow, and con-
trolling its direction and shape” [2].
So to speak, a nozzle is a duct with cross section area A, which varies
along the direction of the flow, x : A = A(x).
As the flow in the nozzle is considered to move essentially in one direction,
x, rapidly, and its average velocity u(x) > 0, we can make a first approxi-
mation as uni-dimensional and adiabatic, thus the ideal or isentropic model
is applicable throughout the nozzle. Later on, the isentropic model equa-
tions will be reviewed. The variables are measured as a section-average:
M(x), p(x), ρ(x), T(x).
1

Figure 1.1: Scheme of a CD Nozzle.
We have considered that the flow is isentropic. Also, we take into account
the case of a steady flow. Afterwards, as our flow is in a steady state, the
mas flow rate Q = ρuA remains constant. Added to it, we consider the
momentum conservation, perform a sum of forces in the x direction, and
note that the flow has a compressible nature. A trivial development (which
is not the objective of this thesis), leads us to the equation which explains
the fundamental behaviour of the compressible flow in a duct with variable
cross-section:
(M2
− 1)
1
u
du
dx
=
1
A
dA
dx
(1.1)
According to the given definition of nozzle, we could consider three sce-
narios depending on whether the cross-section is increasing, decreasing or
stays constant. Thus, we will regard two types of nozzles: convergent, C,
(increasing area), and convergent-divergent, CD, (decreasing area). The last
case refers to a straight duct with constant area.
Convergent Nozzles
A convergent nozzle is a duct with a locally decreasing area (dA
dx
< 0).
Depending on the velocity u of the inflow:
– Subsonic case (M < 1): the flow accelerates (du
dx
> 0).
– Supersonic case (M > 1): the flow decelerates (du
dx
< 0).
Since the inflow considered is subsonic, the discharge pressure, or the
pressure at the exit of the nozzle will be the same as the ambient (pe = p∞).
2

A convergent nozzle can only reach supersonic conditions (M = 1) at the
exit of the nozzle, which means that the flow is choked, so (pe = p∞). This
will result in a series of expansion waves and oblique shocks that accommo-
date the pressure to the free-stream one, which will be reviewed later on. A
convergent nozzle will be the object of study of this thesis.
Straight Duct
The case in which the area is neither converging nor diverging (dA
dx
= 0),
is important for us in the sonic case (M = 1). We can have that:
– Sonic case (M = 1): it could happen (du
dx
< 0), (du
dx
> 0) or even
(du
dx
= 0).
Therefore, the very end of a nozzle or the throat section can be consid-
ered as an infinitesimally straight duct. They are the only regions where
sonic conditions can be reached. Furthermore, as mentioned, the object of
this thesis is a convergent nozzle. Thus, it can reach sonic conditions at the
end of it if choked.
Convergent-Divergent Nozzles
A CD nozzle is a duct with locally increasing area (dA
dx
> 0). Depending
on the velocity u of the inflow:
– Subsonic case (M < 1): the flow decelerates (du
dx
< 0).
– Supersonic case (M > 1): the flow accelerates (du
dx
> 0).
A CD nozzle is the only way to obtain a supersonic flow (M > 1) when
choked (M = 1 at the throat area). It presents a more complex behaviour, as
shock waves and expansion fans can be formed inside or outside of the nozzle.
1.1.1 Modes of Operation
Firstly, there are several considerations that need to be made. We are look-
ing at a CD nozzle, as in Fig. 1.1. The nozzle is connected to a reservoir
at the stagnation (total) conditions, T0, p0. The nozzle discharges at the at-
mosphere, which is at rest, thus having a static pressure p∞. The exit static
pressure considered, at the very end of the CD nozzle (divergent part, Ae),
3

is pe.
Accordingly, depending on the exit pressure, we will have several cases
(see [4]):
• Flow subsonic at the exit (Me < 1): the exit pressure will be the same
as the ambient (pe = p∞). This will be the case of a C nozzle, too.
• Flow supersonic at the exit (Me > 1): there are three possibilities.
– If (pe = p∞). Perfect harmony.
– If (pe > p∞). We say that the ﬂow is ”under-expanded”. It means
that the exit pressure is not low enough to match that of the
ambient, thus, a series of expansion fans need to appear in order
to reach ambient pressure, after exhaust.
– If (pe < p∞). We say that the ﬂow is ”over-expanded”. It means
that the exit pressure is lower than the ambient one, therefore,
oblique shocks need to take place in order to adapt to the ambient
pressure, after exhaust.
Figure 1.2: Behaviour of a CD Nozzle depending on the exit pressure with
respect to the ambient pressure.
4

To expand on this point, as we are looking at a CD nozzle, in order to
obtain a supersonic flow at the exit, the nozzle needs to be choked. It means
that, at the throat area (see Fig. 1.1), denoted t, the flow is sonic (Mt = 1),
and maximum mass flow rate Q is reached.
In Fig 1.3 we can observe the different modes of operation as a function
of the pressure ratio p/p0.
1. The flow in the nozzle is subsonic everywhere (pe = p∞, Me < 1).
Therefore, we have that (Mt < 1).
2. The flow is choked (Mt = 1), but subsonic downstream (Me < 1).
Thus, we get (pe = p∞).
3. The flow is choked (Mt = 1) and supersonic downstream (Me > 1).
There are, depending on the exit pressure, various options:
(a) pe > p∞: the mentioned ”under-expanded” case. A series of ex-
pansion fans appear.
(b) pe = p∞: perfect harmony. This is usually the on-design case.
(c) pe < p∞: by using the normal shock relationships, we obtain
that a weaker compression than a normal shock needs to appear
(through oblique shocks).
(d) pe < p∞: by using the normal shock relationships, we obtain that
the pressure just after the shock is that of the ambient. Therefore,
we have a normal shock at the exit.
4. The flow is choked (Mt = 1), and supersonic downstream. However, by
using the isentropic relationships and normal shock relationships, we
obtain that a normal shock needs to appear within the nozzle, in order
to have pe = p∞.
5

Figure 1.3: Modes of operation of a CD Nozzle as a function of the pressure
ratio p/p0. [4]
Figure 1.4: Modes of operation of a CD Nozzle as a function of the Mach
number M. [4]
6

1.2 Description of the Exhaust Jet in a C and
CD Nozzle
We have considered an isentropic, steady-state, 1-D, axisymmetric flow. Fur-
thermore, we consider an ideal gas (air). The following governing equations
define it [5]:
Continuity:
ρ1u1A1 = ρ2u2A2 (1.2)
Momentum:
p1A1 + ρ1(u1)2
A1 +
A2
A1
pdA = p2A2 + p2(u2)2
A2 (1.3)
Energy:
h1 +
(u1)2
2
= h2 +
(u2)2
2
(1.4)
Perfect Gas:
p = ρRT (1.5)
Calorically Perfect Gas:
h = cpT (1.6)
By developing Equations (1.2) to (1.6), we find that the evolution of the
Mach number along the nozzle is a function of the Area ratio A/A∗
:
A
A∗
2
=
1
M2
2
γ + 1
1 +
γ − 1
2
( γ+1
γ−1
)
(1.7)
It all leads us to the obtainment of the isentropic 1-D relationships of the
nozzle flow.
p0
p
= 1 +
γ − 1
2
M2
γ
γ−1
(1.8)
ρ0
ρ
= 1 +
γ − 1
2
M2
1
γ−1
(1.9)
T0
T
= 1 +
γ − 1
2
M2
(1.10)
7

c0
c
= 1 +
γ − 1
2
M2
1
2
(1.11)
1.2.1 Structure of the Jet
The kind of flow that we are going to look at is a free shear flow, more specif-
ically a supersonic jet. The name free shear flow [1], [7], implies that these
flows are not interacting with any wall or surface, and that the turbulence
that we observe comes mainly from a mean-velocity difference. These phe-
nomena is exactly what is happening in the exhaust jet studied.
Whether it comes from a C or a CD nozzle, the structure of the jet has
common general features [6], that we can divide into three regions, shown
in Fig. 1.5. The specific case studied in this thesis is a supersonic under-
expanded flow coming from a C nozzle, as we will later study.
In the near-field zone, we can find two parts, 1 and 2. Part 1 corresponds
to the potential core, and part 2 to the mixing region. The potential core is
delimited by the confluence of two mixing-layers that develop from the trail-
ing edge of the nozzle. The potential core is isolated from its surroundings,
which means that its behaviour is dominated by compressible effects. In sec-
tion 1.2.2 we will further explain the phenomena that the flow undergoes in
the potential core. In the mixing region, the turbulence generated induces
an exchange between the exhaust jet and the ambient air.
The transition zone refers to a region where variations in the properties
of the flow start getting smaller, and the exhaust jet and the surrounding air
have more similar properties.
Finally, in part 3, the far-field zone, downstream, the jet is fully-expanded,
developed, and reaches a self-similar state.
The length of the potential core is strongly influenced by the difference
between the exhaust and external pressure. Therefore, to study the phenom-
ena that occurs in the potential core, it is very important if the supersonic
jet is over, under or fully-expanded.
8

Figure 1.5: Schematic representation of the structure of an under-expanded
jet. [6]
1.2.2 Shock Diamonds and Mach Disks
Now that we have reviewed the C and CD nozzles, it is clear to see why CD
nozzles are used for supersonic applications, such as rockets, missiles and
supersonic aircraft.
We also know that the exhaust pressure of a supersonic jet, in a real-life
scenario, can be adjusted. The goal is, in a CD nozzle (such as the ones in
fighter jets or rockets), to optimise the thrust in function of the altitude and
speed. As seen in Eq. (1.7), the Mach number depends on the area ratio,
which means that our exit Mach number, Me, will vary if we vary this ratio.
In practice, the only way to modify it, is by changing the exit are Ae, with
a variable area nozzle. An example is found in fighter aircraft, in Fig. (1.6).
In the case of rockets, the bell-shaped nozzles have a fixed area. Thus, it
is impossible to change the area (see Fig. 1.7 ). However, and experimental
engine has been tested, called the Aerospike, which has a cone-shaped nozzle,
without external walls, which allows the flow to self-adjust to the external
pressure (see Fig. 1.8).
9

Figure 1.6: Petals or ”Turkey feathers” of a variable area nozzle in a Eu-
roﬁghter Typhoon EF2000.
Figure 1.7: Nozzle of the Aerojet Rocketdyne RS-25, also known as the Space
Shuttle main engine (SSME).
10

Figure 1.8: XRS-2200 linear Aerospike Engine Nozzle for the X-33 program.
In section 1.2.1 we have stated that, within the potential core region, there
are characteristic phenomena that the flow undergoes. We will focus on an
under-expanded flow, as it is the one studied specifically in this thesis. In sec-
tion 1.1.1 we have stated that the flow must adapt to the ambient conditions.
As the flow is under-expanded, we have an exit pressure higher than the
ambient pressure. Therefore, a series of expansion fans develop, making the
flow turn outwards and reduce its pressure [3]. As we can see in Fig. 1.9, the
expansion fans meet their symmetric counter-parts at the center line, and
bounce off to the jet boundary. The flow must not cross the center line, as
it is a symmetry line, wall-like.
Now, the expansion fans reflect off the free jet boundary, towards the
center line. Again, these expansion fans reflect once more and make the flow
turn inwards. It creates a compression fan that increases the pressure of the
flow. If strong enough, these compression fans will merge into an oblique
shock and form a Mach disk. These oblique shocks rise the pressure of the
flow, forcing the creation of a new series of expansion fans, and so the pro-
cess begins again, repeating itself creating a series of Mach disks and Mach
diamonds in the exhaust, until the exit pressure matches the ambient one.
These Mach disks and diamonds are clearly seen in supersonic engines, as
11

we can see in Fig. 1.7, Fig. 1.11, Fig. 1.12 and Fig. 1.13. We can clearly
observe the formation of a pattern of disks or cones of a lighter colour, as
predicted.
A similar process will occur in the case of an over-expanded jet (see Fig.
1.10 . Nonetheless, in this case, the exit pressure is lower than the ambient.
Oblique shocks will form at the trailing edge of the nozzle, and we will get
an identical sequence of expansion fans and oblique shocks (as for an under-
expanded nozzle).
Figure 1.9: Wave structures that create shock diamonds in an under-
expanded ﬂow. [3]
Figure 1.10: Wave structures that create shock diamonds in an over-expanded
ﬂow. [3]
12

Figure 1.11: Mach diamonds structure in the J58 engine of the SR-71 ”Black-
bird” running with afterburner.
Figure 1.12: Mach diamonds structure in a F-15 Eagle.
Figure 1.13: Mach diamonds structure in a F-16 Falcon.
13

A brief summary of the phenomena occurring at the trailing edge of a CD
nozzle is presented in Fig. 1.14. Depending on the exit pressure, if the flow
is over-expanded (as in Fig. 1.10), oblique shocks will form at the trailing
edge of the nozzle, and the flow will be forced to turn inwards. Secondly,
if the exit pressure perfectly matches the ambient pressure, no expansion or
compression will be formed. The direction of the flow remains unchanged.
This is the ideal case. Finally, if the flow is under-expanded, a series of
expansion fans will appear. The flow will turn outwards (as in Fig. 1.9).
Figure 1.14: Summary of the phenomena at the trailing edge of a nozzle in
function of the exit pressure.
14

1.3 CFD-TAU
In this section, we will be introducing the field of CFD and a general review.
Secondly, we will be studying the DLR TAU-Code R
, which is the one used
in this thesis to carry out the numerical simulations in order to solve the
flow; developed by the DLR, German Institute for Aerodynamics and Flow
Technology.
1.3.1 Computational Fluid Dynamics Overview
CFD can be considered as a branch of fluid mechanics that uses numer-
ical analysis to solve problems that involve fluid flows. It also integrates
the disciplines of mathematics (the physical characteristics of the flow can
be described through mathematical expressions) and computer science (the
mathematical expressions are converted into programming languages to be
solved by computers).
CFD is as a tool complementary to experimental and theoretical meth-
ods (such as wind tunnels and flight tests) available to solve fluid-dynamic
and heat transfer problems. CFD can be used in a wide variety of fields.
For instance, biomedical purposes (the flow of blood through our vascular
system) or weather simulations. However, on this thesis, it is clear that we
will be focusing on the aerospace analysis applications of CFD.
The basis of CFD, as for standard fluid mechanics, are the Navier −
Stokes Equations (very difficult to solve). Obviously, depending on the na-
ture of the flow, we can simplify these equations, obtaining the Euler Equa-
tions, for adiabatic, inviscid flows.
As mentioned before, the Navier − Stokes Equations, have been proven
to be very difficult to solve. Nonetheless, CFD offers us an alternative to
obtain solutions to these problems, by always following a general procedure
(see Fig. 1.15).
Preprocessing
• The physical boundaries and the fluid domain of our problem are de-
fined. It is usually done using CAD geometry.
The problem that this thesis tackles, as we will later study, uses the
15

CAD geometry of a C nozzle. It was provided by a research team at
the Université de Poitiers.
• The fluid domain is divided into discrete cells, creating a mesh.
This thesis deals with a 2D domain. The meshes that we will be con-
sidering, are either structured (uniformly distributed cartesian mesh)
or unstructured (no regularity to the arrangement of the cells), and use
triangular or quadrilateral elements. These two types will be studied
more in depth in Section 2, using the specific meshes of this thesis (see
examples in Fig. 1.16 and Fig 1.17).
As mentioned, the domain needs to be discrete. There are several
discretization methods used today for CFD. However, for practical
purposes, as it is simple to apply, widely used in CFD and it is the
method used in the DLR TAU-Code R
, in Section 1.3.2, we will focus
on the finite-volume method.
• Boundaries are defined, and boundary conditions specified. It refers to
the behaviour of the fluid at the boundaries of the fluid domain. It will
be reviewed, for this thesis, in Section 2.
• The mathematical expressions that define the physical state of the flow
are defined. In general terms, the three main equations are Continuity,
Momentum and Energy. Furthermore, we will be performing numerical
simulations on turbulent flows, RANS simulations, on this thesis. Two
more equations need to be added in order to compute the turbulent
model. The k- Two Equation Turbulence Model will be used. More
in depth in Section 3.
Solver
The numerical simulation is computed by the DLR TAU-Code R
. The
three mentioned governing equations are solved, added to the two equations
coming from the chosen turbulence model. Obviously, there are other equa-
tions involved, such as the equation of state and calorically perfect gas.
The simulation runs until the desired steady-state is reached.
Postprocessing
Finally, after a solution has been obtained, we need to visualize the re-
sults. In our case, the software Paraview is used. We build visualizations to
analyze data using qualitative and quantitative techniques.
16

Figure 1.15: The three main elements of a CFD analysis. [13]
Figure 1.16: Example of a structured mesh. [13]
17

Figure 1.17: Example of an ustructured mesh. [13]
1.3.2 The DLR TAU-Code R
The DLR TAU-Code R
[13] is a CFD-tool for complex configurations sim-
ulated with hybrid unstructured grids. We have to clarify that TAU does
not include a grid generation module. However, it does include modules for
grid adaptation and modification (explained below). TAU can be used with
either structured or unstructured meshes, composed, in our 2D case, of tri-
angular and quadrilateral elements. TAU is a modern software system used
for the prediction of viscous and inviscid flows from the low subsonic to the
hypersonic flow regime.
In the previous section, we mentioned that the fluid domain needs a dis-
cretization. TAU is a second order finite volume flow solver. We will explain
more in depth this discretization method used in the code.
Finite Volume Method
The finite volume method discretizes the integral form of the conserva-
tion equations directly in the physical space. ”The computational domain
is subdivided into a finite number of contiguous control volumes, where the
resulting statements express the exact conservation of relevant properties for
each of the control volumes. At the centroid of each of the control volumes,
the variable values are calculated” [13]. It can be applied for both, a two and
a three-dimensional domain.
So to speak, we are dividing our fluid domain in small volumes, adapting our
governing equations to these volumes, solving them and obtaining a solution
for our physical properties at the centroid of the control volumes (see Fig.
1.18).
TAU solves either RANS equations or Euler equations only.
18

Figure 1.18: Representation of the ﬁnite volume method for a structured and
unstructured grid. [13]
Modules
The TAU package has several main modules:
• Grid Partitioning.
The grids are partitioned in the requested number of domains at the
start of the simulation. In the case of this thesis, the number of domains
selected is one. However, multiple domains can be chosen, in case
parallel computations are performed (multiple CPUs; see Figure 1.19).
Figure 1.19: Example of multiple domains of TAU parallel grid partitioning.
[11]
• Preprocessing.
The pre-processing needs to be employed once for a given primary grid.
It computes the dual grid composed of general control volumes from
19

the primary elements. It makes the solver independent of the cell types
of the primary grid. The number of multigrid levels can be chosen. In
the case of this thesis, we have chosen three multigrid levels.
Figure 1.20: Example of the TAU preprocessor dual grid approach. [11]
Figure 1.21: Example of the TAU preprocessor number of multigrid levels.
[11]
• Flow solver.
The TAU ﬂow solver uses, when it comes to physical models, com-
pressible RANS equations.
As for the numerical methods, we have already mentioned that TAU
uses a second order finite volume discretization method. Moreover,
inviscid terms are computed using either second order central schemes
(chosen for our thesis) or upwind schemes. Viscous terms are computed
with a second-order central scheme. Also, a scalar or matrix artiﬁcial
dissipation scheme can be chosen (scalar in our case).
20

Time integration is performed through either a explicit Runge−Kutta
or implicit LUSGS scheme. In this thesis, the LUSGS scheme is se-
lected, as it presents several advantages.
• Grid Adaptation.
In order to be able to solve very detailed flow features, TAU performs
a grid adaptation, based on a local grid refinement (see Fig. 1.22).
Figure 1.22: Example of TAU grid adaptation. Local grid refinement. [11]
• Grid Deformation.
TAU includes a grid deformation tool. It takes into account the de-
formations of surfaces due to the structural analysis, as a response to
the different loads that our system is under (for instance, aerodynamic
loads). An example is shown in Fig. 1.23.
Figure 1.23: Example of TAU grid deformation. Deflection of the tip of a
wing of an aircraft. [11]
21

In this section, we have presented a general review of the features of the
TAU code. Moreover, we have stated that many of the parameters mentioned
can be chosen by the user. It is selected via the input TAU parameter file,
created by the user, which will be explained more in depth in the following
sections.
1.4 Objectives and Structure of this Thesis
This thesis has been conducted alongside the E.T.S.I.A.E. Applied Math-
ematics Department. It owns some high-computational resources that are
shared among the researchers and students working at the department. It
is called ”Bender”. Thanks to it, it was possible to perform the numerical
simulations needed in order to obtain the desired results.
This has been a pioneering thesis on this specific subject. It is the first
thesis done in the Department, using the TAU code. It has opened a new
research path for future students to continue developing it, and use the in-
formation obtained in this thesis to help them get through the issues that
arise in the first stages.
In the long term, the objective is to obtain a reliable RANS simulation
that will give us an accurate mean flux. From it, we will be able to get a
consistent velocity field, which describes precisely the behaviour of the tur-
bulent supersonic jet, coming out of the nozzle. Currently, on this thesis,
we are using a C nozzle, and a single jet. However, if more students keep
developing it, we will reach the final goal, a twin-jet configuration for both,
C and CD nozzles.
The mentioned velocity field allows us to explain the compressible effects
within the potential core of our jet. Furthermore, it describes the phenom-
ena that occurs within; the formation of a series of mach diamonds and disks.
Considering the amount of resources available, that this thesis has been
started from scratch, and that it is carried out by a single student, it is a far-
fetched assumption to think that the long-term objectives could be achieved.
Therefore, a more realistic approach for this thesis has to be considered.
The short-term objective (and the objective of this thesis) is, firstly, to
establish a ”recipe” for future students to follow. It contains the steps needed
to get from the CAD geometry provided, generate a mesh, convert it into a
22

TAU format and run the simulations, and finally observe the solutions.
Secondly, as mentioned before, it explains the solutions to many issues
that arise in the first stages, and that have already been solved. It is, thus, a
paper to refer to, in case information is needed for the basics of this problem,
should an issue appear.
Finally, numerical simulations have been performed. RANS simulations
on a supersonic jet. We have obtained solutions for different meshes (struc-
tured and unstructured), with and without nozzle, and for different degrees
of refinement. This has allowed us to compare the solutions obtained, and
make suggestions of improvement for future ways of optimization. Future
students could always refer to this thesis to look for ways of improving their
work, and which path to take.
When it comes to the structure of this thesis, it follows a clear route, as
it is shown in the Contents index.
In first place, a general review on supersonic jets and nozzles is presented.
We get a general understanding of what is happening in the exterior flow and
in the nozzle flow. The structure of the jet itself is explained, and the phe-
nomena that happens within. On this point, the last step is to make an
overview of CFD and the specific TAU code used in this thesis.
Secondly, the three clear steps to follow on a CFD problem are presented:
pre-precessing, solver, and post-processor. These three points are solved for
the specific CFD task tackled in this thesis. The software used is presented,
how we have worked with it, which path has been followed, which problems
have been solved.
Finally, and a very important point for future students, suggestions on
improvements for this work are made. Predictions on what might work best
are shown, relying on the experience acquired throughout the development
of this paper.
23

Chapter 2
Pre-processing: from CAD
Geometry to Mesh
2.1 Scheme of the Process
One of the objectives of this thesis is to create a ”recipe” for future stu-
dents to use as a guideline for their work. This section focuses on the
pre − processing part of the CFD problem. It goes from the very first
step, the given CAD geometry, to the extraction of a suitable mesh format
for TAU to compute.
We have to clarify that, to start with, the CAD geometry used was given
by the Université de Poitiers. A research team in this university carried out
various experiments using nozzles of different shapes. The nozzle used in this
thesis is the C Nozzle provided by them (see Fig. 2.1).
Furthermore, in section 4 we will be using the results obtained by the
Université de Poitiers and comparing them to the ones obtained in this the-
sis. Nonetheless, we have to take into account that the results provided by
the Poitiers team, were obtained via hot-wire measurements, and not nu-
merical simulations. Therefore, the nature of the experiment is very different.
We are trying to replicate an empirical experiment through a CFD analy-
sis, which is quite a feat considering the magnitude of the project and the
resources available. Conclusively, the results presented in section 4 have to
be carefully analysed and interpreted.
The following colour scheme summarises the steps to follow and the soft-
ware used in each of the steps:
25

Step 1
CAD geometry of a C
Nozzle. Provided by
Université de Poitiers
Step 2
Extract Nozzle 2D contour
using ANSYS SpaceClaim R
Step 3
Create fluid 2D do-
main geometry using
ANSYS SpaceClaim R
Step 4
Create 2D mesh us-
ing ANSYS Mesher R
Step 5
Edit 2D mesh and ob-
tain 3D mesh using
ANSYS ICEM-CFD R
Step 6
Export 3D mesh from
ANSYS ICEM-CFD R
to a
format compatible with TAU
Step 7
In Bender transform
ANSYS ICEM-CFD R
mesh
format to TAU format mesh
Step 8
In Bender from 3D TAU
mesh obtain a 2D TAU
mesh to feed TAU solver
,
2.2 Extraction of the Geometry of the Nozzle
In this section, we will be explaining, from the colour scheme, step 1, step 2
and step 3.
Step 1
In Fig. 2.1 we can observe the 3D CAD C nozzle provided by the Univer-
sité de Poitiers. It is the nozzle whose profile has been extracted to be part
of the fluid domain. It is used for the numerical simulations of this thesis.
26

Figure 2.1: Views from diﬀerent perspectives of the C nozzle used in this
thesis.
Step 2
The proﬁle of the C nozzle is extracted using ANSYS SpaceClaim R
.
We insert the 3D CAD nozzle provided (format ”.stl”) into the SpaceClaim
module. The nozzle is axisymmetric. It revolves around the x axis. It means
that, for practical purposes, as it is symmetric, we will only be considering
”one half” of the nozzle, saving computation time. The contour of the nozzle
is shown in Fig. 2.2.
Figure 2.2: Contour of the C nozzle used, extracted in SpaceClaim.
27

Furthermore, as it is an experimental nozzle, it has what we would con-
sider as a ”small” size, compared to, for instance, a typical combat aircraft
or rocket nozzle. The following measurements are expressed in millimeters
(mm):
Figure 2.3: Measurements of the C nozzle expressed in millimeters.
Now, looking at the measurements, we focus on the measurement that
goes from the inner bottom part of the nozzle to the symmetry axis (in red
12,7 mm). It refers to the internal diameter of the nozzle. As mentioned, it is
symmetric, and we will only be taking into account one ”half” of the nozzle.
Thus, we have two diameters to look at. Firstly, there is the entry diameter
(64,77 mm). Secondly, there is the exit diameter (12,7 mm). However, for
calculations, we will be considering the actual diameters of the nozzle (which
means two times the mentioned diameters, both ”halves”). Finally, as it will
be explained later, the reference diameter D, will be the actual exit diameter
(25,4 mm).
Step 3
This step consists of the creation of the fluid domain using ANSYS Space-
Claim R
. This domain will be later used to serve as the basis of the mesh to
generate.
We have mentioned before that two main types of meshes will be used:
structured and unstructured. There is a reason why these types of meshes
are mentioned at this point. It is because the generation of the geometry of
the fluid domain, must be focused on adjusting to the type of mesh to gen-
erate. Furthermore, for analysis reasons, another two types of fluid domains
have been created: with and without the geometry of the nozzle included, as
we will see below. It will be used to compare the results obtained by both of
the domains.
28

To expand on this point, in Fig 2.4, we can observe the general measure-
ments of the domain from which all the other domains start. They refer to
the exit diameter D.
Figure 2.4: General measurements of the Fluid Domain.
• Structured Domain
The objective is to divide the ﬂuid domain into smaller quadrilateral
faces. It is very important that these faces have a quadrilateral-shape,
as much as possible. If not, the software will not read the domain cor-
rectly, and the mesh generation will not be adequate.
In this case, 61 faces were created (see Fig. 2.5). The most complicated
region is the one where the curvature of the nozzle meets the free ﬂow.
As we can observe, this domain has the geometry of the nozzle included.
In Fig 2.6, we have zoomed into the nozzle geometry region. We can
observe that, ”attached” to the nozzle itself, there is a rectangle-shaped
face, at the beginning. This region has been added to make easier
the application of boundary conditions, simulating a straight duct or
reservoir. This way, we avoid the possibility of inconsistencies in the
boundary conditions, if applied directly beside the region where the
curvature of the nozzle begins.
29

• Unstructured Domain
The unstructured domain has been created starting from the regions
already drawn for the structured mesh, and modifying them. We end
up with larger faces. They do not need to resemble exactly a quadri-
lateral shape. These faces could be regarded as areas of ”inﬂuence”,
where a reﬁnement is going to be performed (see Fig. 2.7).
Moreover, in Fig. 2.8, as for the structured mesh, a detailed view is
shown. It follows the same pattern as the structured mesh.
Figure 2.5: Fluid Domain for a Structured Mesh.
Figure 2.6: Detailed view of the nozzle geometry region of the structured
domain.
30

Figure 2.7: Fluid Domain for an Unstructured Mesh.
Figure 2.8: Detailed view of the nozzle geometry region of the unstructured
domain.
• Domain without Nozzle
Finally, as mentioned before, we have created as well domains without
nozzle. The same domain is used. However, the nozzle geometry region
is removed, and a small ”lip” or ”ﬂap” is created where the nozzle
was. This has been done as a solution to correctly apply the desired
boundary conditions (see Fig. 2.9 and Fig. 2.10).
31

Figure 2.9: Geometry of fluid domain without nozzle.
Figure 2.10: Detailed view of the region of the domain without nozzle.
2.3 Generation of the 2D Meshes
In this section, we will be explaining, from the colour scheme, step 4, step 5
and step 6.
Step 4
Using ANSYS Mesher R
, we will be meshing the fluid domains mentioned.
Starting from the ones mentioned above, we end up with four different types
of meshes:
32

– Structured mesh with nozzle geometry.
– Structured mesh without nozzle geometry.
– Unstructured mesh with nozzle geometry.
– Unstructured mesh without nozzle geometry.
Furthermore, we will be applying a second refinement to the meshes
above. It is useful to compare the different results obtained and check the
degree of refinement needed in order to have a good quality mesh.
To expand on this point, the following meshes were created from zero,
using the geometry of the fluid domains. Again, it is a first approach, as
there are no other meshes to compare to. The results obtained can be used
to guide future students, and generate better quality meshes.
Figure 2.11: Structured mesh with nozzle geometry.
Figure 2.12: Structured mesh with nozzle geometry. Detailed view.
33

Figure 2.13: Structured mesh with nozzle geometry. Detailed view.
Figure 2.14: Unstructured mesh with nozzle geometry.
Figure 2.15: Unstructured mesh with nozzle geometry. Detailed view.
34

The meshes generated without the nozzle geometry, follow the exact same
mesh pattern. However, the nozzle geometry part has been removed.
Moreover, in order to obtain the above meshes, the following tools of
ANSYS Mesher R
have been used, combined with the modification of the
general parameters of the mesh:
– Face meshing.
– Edge sizing.
– Method.
– Refinement.
To finish with, we export the 2D mesh to an ICEM − CFD compatible
format. In this case, it is the ICEM-CFD input file, a ”.prj” format.
Step 5
Using ANSYS ICEM-CFD R
, we edit the 2D mesh, extrude it, and obtain
a 3D mesh. The mesh is, in the first place, generated on the xz plane, and
later extruded on the y axis. In Fig. 2.16, we present an example of the 3D
mesh generated.
Figure 2.16: Example of a 3D extruded mesh.
At this point, in ANSYS ICEM-CFD R
, we have to define some param-
eters to be used in the parameter file. We are going to set the ”Boundary
Mapping File”, one of the sections of the TAU parameter file. This way,
boundary conditions are selected.
35

In the mentioned 3D mesh, we have to select the desired surfaces. In Fig.
2.17, for a better understanding, it is shown on the 2D xz plane. After they
have been selected, TAU assigns them a marker, which will be later used to
process the mesh in Bender. The boundary conditions applied to the above
mentioned surfaces, will be later explained, in section 3.2. The names given
to the surfaces are deﬁned by the user.
– INLET: 1
– TOP INLET: 2
– SYMMETRY SIDE: 3 (there are two of this surfaces, on either side of
the mesh).
– TOP WALL: 4
– NOZZLE WALL: 5 (only present in the mesh with nozzle geometry).
– SYMMETRY AXIS: 6
– OUTLET: 7
– INLET WALL: 8
– END NOZZLE DUCT: 9 (the mentioned ”lip” present in the geometry
without nozzle).
Figure 2.17: Example of the markers used for the mesh with nozzle geometry.
36

Figure 2.18: Example of the markers used for the mesh without nozzle ge-
ometry .
Step 6
From ANSYS ICEM-CFD R
, we simply export the 3D mesh generated,
to a compatible format with TAU. The format is ”.uns”, which will be later
read using Bender.
2.4 Export to a TAU Format Mesh
In this section, we will be explaining, from the colour scheme, step 7 and step
8.
Step 7
We will use now the mentioned Bender. Through an VPN (in this case
we will be using FortiClient VPN, provided by Universidad Politécnica de
Madrid, and using remote computing (using MobaXterm), we connect to
Bender.
Firstly, via the module icem2tau, we transform the ICEM files to TAU
compatible files, ”.mesh”. In this step, it is important to generate a markers
file, in order to know which number has been assigned to which boundary
surface (Fig 2.19). Once this step is done, we can continue to the last one,
which is preparing the meshes for computation of the solution.
37

Figure 2.19: Module icem2tau in Bender.
Step 8
Via the module setup taugrid, we firstly state that we want to manipulate
a 2D mesh (Fig 2.20).
Secondly, we have to extract from the 3D mesh, the 2D mesh to be ma-
nipulated by TAU (Fig. 2.21). As it can be observed, the selection of the
plane xz to create our mesh is not random, as it is one of the options of the
module. Furthermore, we have to select one of the symmetry planes to be
extracted (SYMMETRY SIDE).
Finally, we save the extracted mesh (Fig. 2.22), as the final and definitive
mesh. It is very important to know that, during this process, one of the
SYMMETRY SIDE markers will have changed its number. Thus, in the
parameter file, it will need to be changed.
Figure 2.20: Module setup taugrid in Bender. Step 1 of the process.
38

39

Chapter 3
Solver: Numerical Simulations
Set-Up
3.1 Definition of the Flow Parameters
We are going to define the parameters and dimensionless numbers present in
the parameter file that is fed to TAU. They will be explained with the same
names given by TAU.
• References
– Reference density ρ: 1.22 [ kg
m3 ]
– Reference temperature T: 293 [K]
– Reference pressure p: 102644.82 [Pa]
– Reynolds length (the length D is used): 0.0254 [m]
– Reference Mach number M: 0.9
These reference values are used to make flow parameters dimensionless.
They have been chosen according to the experiment carried out by the
Université de Poitiers, to try to match as much as possible the results
obtained.
• Perfect Gas Thermodynamic
– Gas constant R: 287 [ J
kgK
]
– Gas constant γ: 1.4
41

• Transport coefficients
– Sutherland reference viscosity µ: 1.7894e-05 [ kg
ms
]
– Sutherland reference temperature: 288.15 [K]
– Sutherland constant: 110.4
– Prandtl number: 0.72
– Reynolds number: 528171.13
The Re number is defined as followed:
Re =
ρuD
µ
Where ρ is the reference density, u is the reference Mach number, D is
the Reynolds length, and µ is the Sutherland reference viscosity.
3.2 Boundary Conditions
We have defined before, in Section 2.3 and Section 2.4 the surfaces used
as boundaries and the markers assigned to them. Furthermore, we will ex-
plain [14] the type of boundary chosen for each of the surfaces.
Euler Wall
”Defines a wall without viscous effects” [14]. We have assigned this type of
boundary conditions to both of the SY MMETRY SIDE, NOZZLE WALL,
TOP INLET. Moreover, in the geometry without nozzle, it has been as-
signed to END NOZZLE DUCT.
Symmetry Plane
”Defines a symmetry plane, where the symmetry is handled by projecting
the momentum flow variables onto the symmetry plane” [14]. It has been
chosen for SY MMETRY AXIS.
Farfield
”The farfield is an inflow/outflow boundary far away from the investigated
configuration for external flow. The presence of the configuration should
42

hardly influence the state of the flow variables at the boundary. All gradi-
ents are assumed to be zero and therefore no viscous effects are taken into
account” [14]. It is used for INLET WALL, TOP WALL and OUTLET.
Furthermore, for these three surfaces, we have to specify as well other
values. The temperature (reference), density (reference), and a Mach num-
ber value. This Mach number is defined as the velocity of the co − flow of
the experiment. Two values have been chosen: ”0.009” and ”0.1”, which will
be explained in depth in the Results section, and the reason why they are
defined like so.
Reservoir-Pressure Inflow
”Defines an inflow boundary for internal flow with prescribed constant
total pressure and total density. The inflow direction is by default perpen-
dicular to each boundary face, or it can be set to a desired direction” [14]. It
is the boundary condition chosen for the INLET, in the case of the geometry
with nozzle.
Two values are to be specified: total density (4 [ kg
m3 ]) and total pressure
(336399 [Pa]). Again, they have been chosen to meet the ones used in the
Poitiers experiment.
Dirichlet
”User defined setting of all values at the boundary” [14]. Now, it is used
for the INLET in the geometry without nozzle. Values of density (2.5 [ kg
m3 ]),
temperature (236.5 [K]) and Mach number (1) are directly set on the bound-
ary.
Now we have no ”deposit” or ”reservoir” in still conditions. The condi-
tions are the ones at the exit of the nozzle. They have been computed from
the results obtained in the case with geometry nozzle.
3.3 Turbulence Model
Throughout history, there have been different strategies devised to solve the
exact Navier-Stokes equations. Turbulence modeling is one of them. It is an
approximation of the mentioned equations. In this thesis, we will be tackling
the RANS approach. In general terms, it follows the below scheme.
43

Firstly, we have a decomposition of the flow variables in to mean and fluc-
tuating parts. Secondly, these terms are introduced into the Navier-Stokes
equations. Finally, there is an averaging of the equations themselves. As a
result, we obtain a term, which is generally referred to as Reynolds stress (the
explanation of the RANS equations is not the objective of this thesis). This
term is unknown. Therefore, it has to be modeled to solve the equations,
and close the problem.
The above problem has led to the creation of many turbulence models.
These models rely on a different number of equations (generally from one to
seven) to solve it. In the case of this thesis, we have chosen a two-equation
turbulence model; k- model. This model is widely used in CFD for solving
of the RANS equations.
In our case, in TAU, this model has to be defined. The k- model used is
the ”two-layer k- ”. According to [14], it is divided in two regions of appli-
cations. However, it is necessary to explain beforehand three other models,
to be able to understand it in general terms.
The following equations are expressed in Einstein notation. Thus, the
subscripts i and j are used for this purpose in this case.
The Wilcox k-ω Turbulence Model
It is a two-equation turbulence model which tries to predict turbulence.
The first equation refers to the variable k, the turbulence kinetic energy.
The second equations refers to the variable ω, which is the specific rate of
dissipation (of the turbulence kinetic energy k into internal thermal energy).
δ(ρk)
δt
+
δ(ρujk)
δxj
= P − β∗
ρωk +
δ µ + σk
ρk
ω
δk
δxj
δxj
(3.1)
δ(ρω)
δt
+
δ(ρujω)
δxj
=
γω
k
P − βρω2
+
δ µ + σω
ρk
ω
δω
δxj
δxj
+
ρσd
ω
δk
δxj
δω
δxj
(3.2)
where
P = τij
δui
δxj
44

τij = µt 2Sij −
2
3
δuk
δxk
δij −
2
3
ρkδij
Sij =
1
2
δui
δxj
+
δuj
δxj
and µt is the turbulent eddy viscosity.
We also have the constants σk, σω, β, β∗
, γ. Depending on the model
(like the following ones), their values will be fixed. However, for this thesis,
only the final values of the constants used will be stated.
The k- Turbulence Model
It is the most commonly used model in CFD. Again, it is a two-equation
model which refers to two variables. The first variable, k, is the turbulent
kinetic energy. The second variable, , refers to the rate of dissipation of
turbulent kinetic energy.
δ(ρk)
δt
+
δ(ρkui)
δxi
=
δ µt
δk
δk
δxj
δxj
+ 2µtEijEij − ρ (3.3)
δ(ρ )
δt
+
δ(ρ ui)
δxi
=
δ µt
δ
δ
δxj
δxj
+ C1
k
2µtEijEij − C2 ρ
2
k
(3.4)
Now, we have the constants to be defined σk, σ , C1 C2 and µt is the
turbulent eddy viscosity.
The Menter Baseline (BSL) Turbulence Model
We come across, again, a two-equation turbulence model. It is a combi-
nation of the k-ω (for inner region of boundary layer) and k- (outer region,
free shear flow) turbulence models.
δ(ρk)
δt
+
δ(ρujk)
δxj
= P − β∗
ρωk +
δ (µ + σkµt) δk
δxj
δxj
(3.5)
δ(ρω)
δt
+
δ(ρujω)
δxj
=
γ
υt
P − βρω2
+
δ (µ + σωµt) δω
δxj
δxj
+ 2(1 − F1)
ρσω2
ω
δk
δxj
δω
δxj
(3.6)
45

where
P = τij
δui
δxj
τij = µt 2Sij −
2
3
δuk
δxk
δij −
2
3
ρkδij
Sij =
1
2
δui
δxj
+
δuj
δxj
and µt is the turbulent eddy viscosity.
The original k-ω turbulence model of Wilcox is used in the sub-layer near
solid walls. The k- model is used in the high-Reynolds-number region. We
are able to perform this division, and blend the two models, by changing the
F1 function of the Menter-BSL model (which can be studied more in depth
online, not in this thesis).
Finally, after definition of the two-equation turbulence model desired in
TAU, the ”two-layer k- ”, we set the following values for the constants:
– σk = 0.500
– σω = 0.400
– βk = 0.090
– βω = 0.070
– γ = 0.556
To conclude, in TAU, there are different solvers that can be used to obtain
the solution of the equations. In our case, we will be using the ”.turb2eq”
solver. It adds the desired extra two equations needed, in order to perform
a proper RANS numerical simulation.
3.4 Numerical Parameters
In the parameter file of TAU, numerous numerical parameters can be user
defined. We will be explaining the most important ones, and the values
to which they have been set. We have to remember that the names given
to them might be different to the conventional ones, as it could have been
46

named differently in TAU.
Main Flux
According to [14], ”this parameter selects the discretization type of the
convective (or “inviscid”) fluxes of the RANS equations”. Usually, for better
stability, the recommended scheme is an ”Upwind”. However, in this thesis,
we have chosen a ”Central” scheme. With the selected numerical parameters
and a ”Central” scheme, the simulation reaches a solution. On the other
hand, if an ”Upwind” scheme is selected, it crashes.
Central Flux
A ”Central dissipation scheme” is selected. It has been set to ”Scalar
dissipation”.
Moreover, we have the ”Central convective mean flow flux”. This param-
eter defines the discretization scheme of the convective fluxes of the mean
flow equations in case of a central scheme for the convective fluxes. It has
been set to ”Average of flux”, which means that the flux is the central aver-
age of the analytic flux on each side of the face.
We have to define as well a ”Central convective turbulence flux”. This
parameter defines the discretization scheme of the convective fluxes of the
turbulence equations in case of a central scheme for the convective fluxes.
We set it as well to ”Average of flux”.
Two important coefficients have to be set. Firstly, a ”second order dissi-
pation coefficient” (generally k2). In combination with other parameters, it
is used for capturing shocks. In our case, it has been set to a value of 100
(being 0.5 the default value). The selected value allows the closure of the
problem. Secondly, the inverse fourth order dissipation coefficient (generally
k4). It is fixed to its default value, 64.
Relaxation Solver
Specifies which method of time-stepping to use. In this thesis, we use a
”Backward Euler” implicit scheme. It is solved via LUSGS iterations. For
the LUSGS iterations, two factors can be modified. They are the ”implicit
over relaxation omega” and the ”implicit over relaxation beta”. These values
have been both set to 0.85. While the simulation works, due to the lack of re-
47

sources and time, the effect of their modification on the simulation is unclear.
Time Step Size
In this section, the general CFL number is selected. It has been found
that this parameter has an enormous effect on the simulation. It has been
set to a value of 0.001. If smaller, the simulation crashes. A hypothesis is
that the time step is not small enough to capture the shocks that appear.
Moreover, two other CFL numbers can be specified. One for the ”coarse
grid” region. It has been set to 0.1. Another one is the CFL number for the
regions where it exists a large gradient of pressure (such as shocks). It allows
us to capture better these shocks. It has been set to 0.001. Again, it affects
greatly the stability of the solution.
Residuals and Tolerances
Residuals, can be regarded as how much our solution deviates from a solu-
tion at each time step. It refers to the convergence of our problem. Generally,
the smaller, the better converged, and a better solution reached. However,
this cannot be the cse. In section 4, their graphs will be presented for the
solutions found. A limit can be set to the residuals, if we want our simulation
to stop running if a certain degree of accuracy is reached. In our case, it is
set to ”10e − 9”, which is never reached. Thus, our simulations stops after
the time steps set by the user.
Tolerances can be regarded, as well, as the level of accuracy reached, or
deviation from a solution. In this case, it is defined for each of the variables,
such as density, temperature or pressure. It has been set to 10e − 12, which
again, is not reached within our solution.
48

Chapter 4
Post-processing: Results
4.1 Description of the Results
We have already gone through all the steps necessary to reach this point. We
have understood, in general terms, the CFD software used, TAU, and how
to implement its parameter file. Moreover, we have created a fluid domain
for the C nozzle used, and we have meshed it using different techniques, to
be compared. Finally, the numerical simulation is carried out, thanks to
Bender. We let it run for the desired time steps, until a solution is reached.
The very last step, as mentioned, is the analysis of the data obtained. We
use Paraview for this purpose.
The Experiment by the Université de Poitiers
Firstly, in this section, we will be presenting the results obtained in the
Poitiers experiment, used as reference. Again, we have to clarify that, in
this experiment, the results shown have been obtained via hot wire.
The Fig. 4.1 shows, in colour, the evolution of the Mach number as a
function of the diameter used as reference. We can observe that it is, as well,
an axisymmetric flow. In this case, both ”halves” are shown. We can clearly
see the Mach diamonds that are formed, the number of shocks, the length
of the potential core (about 12 Diameters), and the mixing region (in lighter
blue).
To expand on this point, a graph of the x velocity profile was provided
(Fig. 4.2). On the y axis, the Mach number. The ”peaks” shown, reflect
the abrupt variation in velocity due to the shocks formed. We can observe 6
49

peaks that correspond to the shocks. Afterwards, there are no more shocks,
and the velocity decreases until it reaches the free stream conditions.
The data that has been used is the following. As NPR, a value of (3.32)
is set. Theoretically, the Mach number at the exit of the nozzle, if a CD
nozzle was to be used, would be (1.430). However, as we are using a C
nozzle, the maximum value that can be reached is (1, sonic conditions). A
reference temperature of (293 [K]). The jet is ﬂowing in ambient pressure
(101325 [Pa]). The jet is considered to be isothermal (constant temperature
after it exits the nozzle).
Figure 4.1: Mach number as a function of the reference diameter, for the
50

Figure 4.2: x velocity profile as a function of the reference diameter, for the
RANS Simulation of a Supersonic Jet
Now, we will be presenting the results obtained for our simulation. After
many simulations, the mesh without the nozzle geometry and unstructured
mesh, has been found to be the most accurate one. The fact that it has no
nozzle geometry included, saves computational time, and the exit conditions
of the nozzle can be set more accurately, as they are defined directly in the
nozzle exit. The data at the exit, has been extracted from the simulations
with the nozzle geometry.
We have already mentioned that a Dirichlet condition is set at the
INLET. The data used is the following: density (2.52 [ kg
m3 ]), temperature
(236.53 [K]), and a Mach number of (1), as it reaches sonic conditions before
the exit of the nozzle.
In Fig. 4.3, we can observe an example of the visualization of the results
in Paraview. For practical purposes, within the software, the ”lower half” of
the solution of our axisymmetric jet is presented. The top left image shows
a general view of the results, and of the fluid domain.
Furthermore, we present the evolution of our solution for different times
51

(for an increasing number of iterations). The image shows, as in Fig. 4.1, the
Mach number colour scheme. Again, we can clearly observe the formation of
the Mach disks and diamonds.
Just from this images, we can say that the number of shocks formed, is
roughly the same as for the Poitiers measurements, 6 shocks.
In Fig. 4.4, a colour scheme of the pressure ﬁeld. It is not as representa-
tive as the Mach number one. However, it is useful to see the areas of greater
pressure created by the shock diamonds, as explained in the theory in section
1.
Figure 4.3: Evolution over time of the supersonic jet. Starting at 10000
iterations (top right), until 50000 iterations (bottom right).
52

Figure 4.4: Colour scheme of the pressure field of our solution for 50000
iterations.
In Fig. 4.3, we can observe, focusing on the coloured region of the Mach
number scheme, that it abruptly stops at one point in the x axis (it is clearly
seen on the top left image, the general view). The reason why the potential
core ”disappears” is explained in Fig. 4.5. It is because of the mesh used.
Due to the magnitude of this research project, as explained, the expectations
of obtaining very accurate data of the mean flux are far-fetched. Thus, we
are focusing on making the simulation work, and obtaining realistic results,
indeed presented. This is why the mesh has been ”shortened”, and only the
potential core region has been refined, to focus on this area.
Figure 4.5: Mesh without nozzle geometry, showing the influence on our
solution. It is focused on the potential core region, where more refinement is
applied.
53

Interpretation of the Results
In Fig. 4.6 (whose counterpart is Fig. 4.2), we find the Mach number
evolution for different times of our simulation. Even though the data might
not be as accurate as we would like it to be, we can see a tendency in the
results as it converges. The importance of this graph relies on the analysis
of the peaks created by the shocks. Their maximum value and distance be-
tween peaks. Nonetheless, there are some points that need to be clarified
beforehand.
The data provided by Université de Poitiers includes: the NPR used,
reference temperature and pressure used during the experiment, and both of
the images provided in this thesis. Thus, we find ourselves in a very limited
position to compare both experiments. The Poitiers experiment serves as a
good reference on how our results should be. However, we are not able to
fully compare numerically both.
On the Poitiers graphs, on the x axis, they represent as a function of the
reference diameter D directly. Whereas us, we represent the value of the x
coordinates. Basically the same value.
On the y axis for Poitiers and our simulation, a Mach number is represented.
As we know, a Mach number is a dimensionless value, that can come from
different expressions. This is one of the issues that arrives in the interpreta-
tion of the results. Due to the lack of information provided, we do not know
how they have obtained their results exactly.
In our case, we can conclude that we are running our simulations consistently.
The difference in the values of the Mach numbers obtained is due to the way
in which we are making properties dimensionless.
In the Poitiers experiment, seemingly, they are using the value Uj (ideally-
expanded jet velocity) to make values dimensionless. This is the velocity that
we would have at the exit of the nozzle, if our exit diameter D was the ideal
one, which would make the nozzle to be choked right at the exit. This value
comes from the isentropic nozzle relations explained in section 1. For us, we
are using the reference Mach number value (M=0.9) to make things dimen-
sionless.
Now that:
– In the experiments, we are measuring the pressure ratio between the
reservoir chamber (where M=0) and the ambient. We are imposing
54

a value of static pressure as boundary condition. Thus, the NPR is
consistent.
– The jets are isothermal, the static temperature is approximately con-
stant and thus, the value of c0 too.
Now, in the data provided by Poitiers, they are using the value U
Uj
to
represent in the y axis of the velocity profile graph. Whereas us, we are using
the value c0 to make the velocity dimensionless. We can conclude that, we
must multiply the values of the Poitiers experiment by the factor Mj =
Uj
c0
.
If we follow the mentioned procedure, results can be compared. For our
experiment, the value of the local jet Mach number Mj for the first peak
obtained (in Fig. 4.6), is around (1.7), which is exactly what is obtained
if we take the Poitiers data and do the above. To expand on this point,
the distance between peaks in our simulations is around (2D). Again, the
Poitiers data confirms our solutions.
To finish with, we conclude that results are consistent, and data of the
shocks formed within the potential core is consistent.
In Fig. 4.7 a graph of the evolution of pressure is presented. It is not
very representative for our purposes. However, they are useful to understand
what is happening inside our jet.
In Fig. 4.8 a graph of the velocity on the x axis. It needs to be scaled
with the reference velocity used, c0.
55

Figure 4.6: Evolution of the Mach Number over time for the mesh without
nozzle geometry.
Figure 4.7: Evolution of the pressure over time for the mesh without nozzle
geometry.
56

Figure 4.8: Evolution of the velocity on the x axis over time for the mesh
without nozzle geometry.
4.2 Mesh Convergence Test
Our goal is to fully run a RANS simulation. It implies reaching a point
in which our simulation is steady (and not a URANS, Unsteady RANS).
While we have not been able to fully run a RANS simulation, our solution
is converging, as shown in Fig. 4.9 via the residuals obtained for the first
refinement meshes, with and without the nozzle geometry. The meshes for
the second refinement follow the same pattern.
While more refinement, apparently, might imply better accuracy, we have
found that it does not mean better results. In the colour scheme graphs of the
Mach number, for a greater refinement, we can see more clearly the shocks
formed. However, our simulation remains unsteady.
57

Figure 4.9: Evolution of the residuals over time. Meshes with and without
the nozzle geometry, and structured and unstructured, first refinement.
Structured Unstructured
With Nozzle 78888 180053
Without Nozzle 77874 237616
Table 4.1: Number of elements for the first refinement meshes.
We have mentioned before that we have used different degrees of refine-
ment to be compared and draw conclusions. They are presented in Table 1
and Table 2. We can observe the number of elements presented in every case
created.
Structured Unstructured
With Nozzle 245102 511059
Without Nozzle 202559 439493
Table 4.2: Number of elements for the second refinement meshes.
Thus, we conclude that the issues within the simulation, not reaching a
steady state, do not come from the meshes themselves (degree of refinement,
geometry), but from the parameter file created (numerical parameters, tur-
bulence model, boundary conditions...).
Furthermore, we have created, within each of the categories of the meshes,
different modifications to try to find out the influence of the geometry of the
58

mesh in our simulations.
In Fig. 4.10, we have ”extended” the region refined for the potential core,
in a straight line. In Fig. 4.11, we have created an ”extended” cone-shaped
mixing region, that grows over the x axis. As we can observe, this last mesh
is very refined.
We can see that neither of them have obtained better results in terms of
reaching a steady state. Furthermore, due to the limited amount of resources
(working on this project with our own personal computer, and running simu-
lations with Bender), the amount of elements that can be used in the meshes
is limited. In the cone-extended mesh, the number of elements created has
reached a point in which the computational time is a bit excessive for a
bachelor thesis project (about a week and a half to be solved). If we were
to run a simulation for each of the times a single parameter is changed, and
observe the solution, it would take too much time to check what influences
the most our solution. Our conclusion is that we must focus mainly on the
TAU parameter file.
To finish with, another parameter that has been taken into account is the
”co-flow”. Whether the ambient air is at rest, or has a certain velocity, it has
to be considered. For our simulations, we have chosen a value of the velocity
co-flow of (co-flow velocity = 0.009Mreference). However, we have observed
that, for our simulations, if other values of co-flow velocity are chosen, such
as (co-flow velocity = 0) or (co-flow velocity = 0.1Mreference), the effects on
the solution cannot be appreciated. Thus, we conclude that, for the moment,
it is not an important parameter.
Figure 4.10: Unstructured mesh, with the potential core region extended and
refined, in a rectangular region.
59

Figure 4.11: Unstructured mesh, with an extended cone-shaped region re-
fined.
4.3 Simulations with and without Nozzle Ge-
ometry
Another strategy devised to find out whether our issues of reaching a steady
state, come from the meshes or the parameters, is running simulations with
and without the nozzle geometry.
Now that the most representative value to be compared, is the Mach
number, in Fig. 4.12 to 4.14, we present their respective values, with and
without the nozzle geometry.
Figure 4.12: Evolution of the Mach number with nozzle geometry, for a
structured and unstructured mesh, and different degrees of refinement.
60

Figure 4.13: Evolution of the Mach number without nozzle geometry, for a
structured and unstructured mesh, and different degrees of refinement.
Figure 4.14: Evolution of the Mach number with and without nozzle ge-
ometry, for a structured and unstructured mesh, and different degrees of
refinement.
Furthermore, we will be presenting a comparison of the results obtained
among the different types of meshes mentioned, structured and unstructured,
and their different degrees of refinement. The structured mesh follows the
geometry shown in Fig. 4.15.
61

Figure 4.15: Example of the structured mesh without nozzle geometry.
Figure 4.16: Example of the results obtained for the mesh with nozzle geome-
try. Top left: first refinement structured mesh. Top right: second refinement
structured mesh. Bottom left: first refinement unstructured mesh. Bottom
right: second refinement unstructured mesh.
Figure 4.17: Example of the results obtained for the mesh without nozzle
geometry. Top left: first refinement structured mesh. Top right: second
refinement structured mesh. Bottom left: first refinement unstructured mesh.
Bottom right: second refinement unstructured mesh.
62

We can clearly observe that the geometry of the mesh aﬀects the solution
too. However, we believe that it is not as essential to reach a steady state as
the parameters selected. Now, if we compare the results obtained, with the
nozzle geometry, with its counterpart without nozzle (presented in section
4.1), we have obtained:
Figure 4.18: Example of the results of the unstructured mesh with nozzle
geometry. Colour scheme of the Mach number for 50000 iterations.
Figure 4.19: Evolution of the Mach number over time, for the unstructured
mesh with nozzle geometry.
We can observe, again, clearly, the shocks formed (in Fig. 4.18). More-
over, in Fig. 4.19 we have the evolution of the Mach number over the x
axis. This time, we get the evolution of the velocity inside the nozzle (at the
beginning). It reaches sonic conditions (M=1) before the exit of the nozzle.
Then, we get the same pattern as for the solution without nozzle, of the
peaks created by the shocks. The ﬂuctuations that we obtain at the end, are
due to the unsteady nature of the solution reached (even if it has converged,
as mentioned).
63

4.4 Mean Flux Characterization
We have already presented all the results obtained. We have concluded that,
in our simulations, we are considering the unstructured mesh, in second re-
ﬁnement degree, as the most accurate one. After analysis of the solution via
Paraview, and comparison with the Poitiers experiment, we have drawn
some conclusions:
– We have six peaks. It means that six shocks (or six mach diamonds)
are created.
– The maximum local Mach number value is around (Mj=1.7), made
dimensionless as mentioned.
– The potential core region extends up to around 19D. It is slightly
larger that the one observed for the Poitiers experiment.
– The distance between peaks is around 2D.
– The jet remains isothermal throughout the free shear ﬂow.
– Values (such as pressure, density, temperature etc.), return to ambient
values far away from the nozzle exit.
– We have not been able to fully capture the mixing region, which is
supposed to grow following a cone-like path (as for the Poitiers exper-
iment). In our experiment, it is seen as a white-ish colour around the
potential core region.
64

Chapter 5
Overview and Conclusions
This thesis will serve as a guide for future students to use. It aims to present
a scheme to follow, to go from a given CAD geometry, process it, run a TAU
simulation and analyse the results obtained.
After a thorough analysis, we have drawn some conclusions. Again, the
goal was never to obtain very accurate results of the mean flux first try.
Indeed, it would have been worrying if seemingly good solutions had been
obtained, regarding the limited amount of time and resources.
On the other hand, some very useful suggestions can be made, for future
students to work on and improve this work:
The meshes used need to be thought more carefully. Now we have some
results to compare with (the ones obtained in this thesis), which we did not
have before. We believe that once the potential core and mixing region are
captured, the mesh is sufficiently accurate. Nonetheless, the transitions be-
tween refinement regions must be made smoother. This affects greatly the
solution, as shown. They need to be more gradual.
Obviously, the parameter file needs to be modified. The boundary condi-
tions used in this thesis, have been found to work and produce a reasonable
solution. Even so, they need to be studied more carefully, and even modified
from its roots, the 3D mesh itself. In the future, after many students have
passed by, a potential non-extruded 3D block mesh could be created, and
boundaries defined more accurately.
Numerical parameters are a crucial part as well. For this thesis, some
aspects have been modified by ”trial and error” to try to find a combination
66

that works. The CFL number must be made smaller. It will save compu-
tational time, and it will probably mean that a more accurate solution is
reached. The numerical solver scheme now used, is a central scheme. Ac-
cording to theory, an upwind scheme is supposed to work better with RANS
simulations. Parameters such as the relaxation factors for the LUSGS iter-
ations, have been left fixed. This could affect the solution too.
We are currently using a ”two-layer k- turbulence model. The coeffi-
cients used are the ones provided by TAU, and have not been changed. This
is an area that could be improved. Potentially, another turbulence model
could be explored, or even a more complex one (three equations or more).
In conclusion, the suggestions made are based on hypothetical areas of
improvement that could lead to a better solution. They are based on the ex-
perience and knowledge acquired with TAU during the six-months research
period of this thesis. Again, very limited time. In the future, all the knowl-
edge gained by the students will be added up, creating a great reference data
base. If this thesis ends as the beginner’s guide of every student who follows
this project, it will have accomplished its goal.
67

Bibliography
[1] Thomas B. Gatski, Jean-Paul Bonnet. (2009). Compressibility, Turbu-
lence and High Speed Flow.
[2] Isidoro Mart´ınez. Nozzles.
http://webserver.dmt.upm.es/ isidoro/bk3/c17/Nozzles.pdf
[3] Aerospaceweb. Shock Diamonds and Mach Disks.
http://www.aerospaceweb.org/question/propulsion/q0224.shtml
[4] Grégoire Winckelmans. Fluid Mechanics and Transfers II: part on com-
pressible flows.
[5] John D. Anderson, Jr. (1995). Computational Fluid Dynamics. The Ba-
sics with Applications.
[6] Erwin Franqueta, Vincent Perrier, Stéphane Gibout, Pascal Bruel.
(2015). Free under-expanded jets in a quiescent medium: A Review.
[7] Stephen B. Pope. (2000). Turbulent Flows.
[8] Gabi Ben-Dor (1992). Shock Wave Reflection Phenomena.
[9] Dieter Schwamborn, Thomas Gerhold, Ralf Heinrich. THE DLR TAU-
CODE: RECENT APPLICATIONS IN RESEARCH AND INDUSTRY.
DLR, Institute for Aerodynamics and Flow Technology.
[10] DLR, Institute for Aerodynamics and Flow Technology.
https://www.dlr.de/as/en/desktopdefault.aspx/
[11] Thomas Gerhold. TAU-Overview.
[12] Computational fluid dynamics.
https://en.wikipedia.org/wiki/Computational fluid dynamics
[13] Jiyuan Tu, Guan-Heng Yeoh, Chaoqun Liu. (2007). Computational Fluid
Dynamics. A Practical Approach.
68

[14] TAU-Code User Guide R
. Release 2013.2.0
[15] NASA. Langley Research Center. Turbulence Modeling Resource.
https://turbmodels.larc.nasa.gov/
[16] 16th AIAA/CEAS Aeroacoustics Conference. Foluso Ladeinde and Ken
Alabi. Tim Colonius and Kristjan Gudmundsson. Robert H. Schlinker and
Ramons A. Reba. An Integrated RANS-PSE-Wave Packet Tool for the
Prediction of Subsonic and Supersonic Jet Noise.
[17] 18th AIAA/CEAS Aeroacoustics Conference. Brès et Al. Unstructured
Large Eddy Simulation of a Hot Supersonic Over-Expanded Jet with
Chevrons.
[18] 20st AIAA/CEAS Aeroacoustics Conference. Brès et Al. Unstructured
Large Eddy Simulations for Nozzle Interior Flow Modeling and Jet Noise
Predictions.
[19] 21st AIAA/CEAS Aeroacoustics Conference. Brès et Al. Large eddy sim-
ulation for jet noise: the importance of getting the boundary layer right.
[20] Andrew T. Thies and Christopher K. W. Tamf. Computation of Turbu-
lent Axisymmetric and Nonaxisymmetric Jet Flows Using the K- Model..
69

Rans Simulation of Supesonic Jets

Recommended

Recommended

More Related Content

Similar to Rans Simulation of Supesonic Jets

Similar to Rans Simulation of Supesonic Jets (20)

Recently uploaded

Recently uploaded (20)

Rans Simulation of Supesonic Jets