ThesisPDF Available

Report ITLR M-Altadill

Authors:

Abstract and Figures

Numerical investigations (2D URANS) of flow past a square cylinder Work Description: External flows past bluff bodies, such as square cylinders, have been studied experimentally very well because of their technical applications. Despite the numerous experimental investigations, numerical simulations of such flows have drawn the interest of many researchers during the last decades. In particular, the accurate prediction of the vortex shedding behind a square cylinder requires robust numerical models, which can yield results for a wide range of geometries and flow parameters, as well as being computational affordable. Currently, large eddy simulations (LES) or direct numerical simulations (DNS) are able to accurately predict these variables. Nevertheless, these methods are mostly limited by the prohibitive computational costs in order to resolve the small-scale turbulent structures. Therefore, unsteady Reynolds averaged Navier-Stokes (URANS) simulations implementing turbulence models are a valuable tool for parameter studies and large engineering problems.
Content may be subject to copyright.
Universität Stuttgart
INSTITUT FÜR THERMODYNAMIK DER LUFT- UND RAUMFAHRT
Direktor: Professor Dr.-Ing. B. Weigand
Pfaffenwaldring 31, 70569 Stuttgart, Germany http://uni-stuttgart.de/itlr
Master thesis
For cand. aer Miquel Altadill Llasat
Numerical investigations (2D URANS) of flow past a
square cylinder
Work Description:
External flows past bluff bodies, such as square cylinders, have been studied experimentally very
well because of their technical applications. Despite the numerous experimental investigations,
numerical simulations of such flows have drawn the interest of many researchers during the last
decades. In particular, the accurate prediction of the vortex shedding behind a square cylinder
requires robust numerical models, which can yield results for a wide range of geometries and flow
parameters, as well as being computational affordable. Currently, large eddy simulations (LES) or
direct numerical simulations (DNS) are able to accurately predict these variables. Nevertheless,
these methods are mostly limited by the prohibitive computational costs in order to resolve the
small-scale turbulent structures. Therefore, unsteady Reynolds averaged Navier-Stokes (URANS)
simulations implementing turbulence models are a valuable tool for parameter studies and large
engineering problems.
Fig.1 Coherent structures in the wake of a square cylinder taken from Trias et al. [1]
[1] Trias, F.Xavier & Gorobets, A. & Oliva, A. “Turbulent flow around a square cylinder at Reynolds number 22,000: A
DNS study”. Computers & Fluids (2015) 123: 87-98
The aim of this work is to investigate to what extend URANS models can predict the turbulent vortex
shedding of the flow around a square cylinder for a Reynolds number Re = 20,000. In addition, an
investigation of the compressibility effects on the coherent structures that develop behind the
square cylinder as well as the importance of the wall resolution will take place. This work ties up on
preliminary investigations at ITLR that can be used as a starting point.
Tasks:
Acquire knowledge of the used software (ANSYS ICEM, ANSSYS CFX, MATLAB)
Acquire knowledge of the relevant flow physics (flow past a square cylinder, URANS
simulation, turbulence modelling)
Literature research on vortex shedding past a square cylinder (most of it will be provided)
Preparation of different numerical grids to study the effect of wall resolution in ANSYS
Evaluation of the numerical results: comparison of the incompressible cases with literature
data, evaluation of compressibility effects
Documentation of the results
Place of work and duration:
This master thesis will be performed at the Institute of Aerospace Thermodynamics. It will be
conducted in cooperation with Prof. Bassam Younis from the University of Davis.
Supervision of the thesis:
Charalampos Alexopoulos, M.Sc., ITLR
Prof. Bassam Younis, Ph.D., UC Davis
Prof. Dr.-Ing. Bernhard Weigand, ITLR
Start date: 15.03.2021
End date: 15.09.2021
Prof. Dr.-Ing. habil. B. Weigand
Hiermit versichere ich, dass ich diese Masterarbeit selbstständig mit Unterstützung des
Betreuers / der Betreuer angefertigt und keine anderen als die angegebenen Quellen
und Hilfsmittel verwendet habe.
Die Arbeit oder wesentliche Bestandteile davon sind weder an dieser noch an einer
anderen Bildungseinrichtung bereits zur Erlangung eines Abschlusses eingereicht
worden.
Ich erkläre weiterhin, bei der Erstellung der Arbeit die einschlägigen Bestimmungen
zum Urheberschutz fremder Beiträge entsprechend den Regeln guter
wissenschaftlicher Praxis eingehalten zu haben. Soweit meine Arbeit fremde Beiträge
(z.B. Bilder, Zeichnungen, Textpassagen etc.) enthält, habe ich diese Beiträge als
solche gekennzeichnet (Zitat, Quellenangabe) und eventuell erforderlich gewordene
Zustimmungen der Urheber zur Nutzung dieser Beiträge in meiner Arbeit eingeholt.
Mir ist bekannt, dass ich im Falle einer schuldhaften Verletzung dieser Pflichten die
daraus entstehenden Konsequenzen zu tragen habe.
……………….……………………………….
Ort, Datum, Unterschrift
Acknowledgments
I would like to thank the following people, without whom I would not have been able
to complete this research, and without whom I would not have made it through my
masters degree. My family, who supported me during all my academic career. My
partner Margalida, I simply could not have done this without you. Finally, my biggest
thanks to my supervisors Prof. Dr.-ing Bernhard Weigand, Prof. Bassam Younis and
M.Sc. Charalampos Alexopoulos for their consistent support and guidance during
the running o this project.
I
Kurzzusammenfassung
Diese Thesis befasst sich mit der Vorhersage des Strömungsfeldes um Vierkantzylin-
der bei einer hohen Reynoldszahl (
Re
= 20
,
000). Die turbulente Natur des Falles
ist eines der Hauptmerkmale der Strömung, da sie zur Bildung einer Kármánschen
Wirbelstraße führt, die erhebliche Schwankungen im Druckfeld bewirkt. Obwohl das
Problem bereits in mehreren numerischen und experimentellen Studien beschrieben
wurde, ist dessen Betrachtung immer noch von Interesse, da so die Einsatzmöglich-
keiten neuer Modelle und Methodiken getestet werden können.
Die Hauptmotivation dieser Arbeit ist es, die Leistungsfähigkeit der instationären
Reynolds-Averaged Navier-Stokes (URANS) Turbulenz-Modellierung zu analysieren.
Dabei wird explizit das Menter
kω
Modell, auch bekannt als Shear Stress Transport
(SST) Modell, angewendet. Durch Gegenüberstellung der Ergebnisse der vorliegenden
Studie und Literaturdaten, können die Stärken und Schwächen des derzeitigen An-
satzes aufgezeigt werden. Die aus dieser ersten Analyse gezogenen Schlussfolgerungen
sind essenziell für den zweiten Teil der Studie, der daraus besteht, den Fall unter
kompressiblen Strömungsbedingungen zu lösen.
Die vorliegende Studie veranschaulicht verschiedene Methodiken, um zu beurteilen,
wie sich die kompressible Natur des Fluids auf die Entwicklung der Wirbelstraße
auswirkt. Nichtsdestotrotz verhindert der Mangel an Daten zu diesem Thema jedoch
einen Vergleich der gewonnenen Ergebnisse.
Schlüsselwörter: Turbulenz
·
Wirbelablösung
·
URANS
·
Mentre
kω·
URANS-SST ·Kompressibilität ·Zweidimensional (2D)
II
Abstract
This thesis focuses on the prediction of the flow field around a square cylinder at a
high Reynolds number (
Re
= 20
,
000). The turbulent nature of the case is one of
the main flow features, since it leads to the formation of a von Kármán vortex street
which yields to significant fluctuations in the pressure field. Although the problem
has been reported in multiple numerical and experimental studies, it is still a case of
interest to test the capabilities of new models and methodologies.
In this work, the main motivation is to analyze the performance of the Unsteady
Reynolds Average Navier-Stokes turbulent-viscosity models. Specifically, the Menter
kω
model, also known as the Shear Stress Transport (SST) model, is applied. By
contrasting the present study results with the literature data it can be proven the
strengths and shortcomings of the current approach. The conclusions extracted from
this first analysis are essential for the second part of the study, which consists on
solving the case under compressible flow conditions.
The present study illustrates different methodologies for assessing how the com-
pressible nature of the fluid affects the vortex street development. Nonetheless, the
lack of data on this topic prevents to contrast the obtained results.
Keywords: Turbulence
·
Vortex shedding
·
URANS
·
Mentre
kω·
URANS-SST
·Compressibility ·Two-dimensional (2D)
III
Contents
Abstract I
List of Tables VI
List of Figures VI
Nomenclature XI
1. Introduction 1
1.1. Motivation ................................. 1
1.2. Scope of the thesis ............................ 1
1.3. Contents description ........................... 2
2. Theoretical Background 3
2.1. Literature Review ............................. 3
2.1.1. Square cylinder case results ................... 5
2.1.1.1. Mean-flow parameters ................. 6
2.1.1.2. Experimental studies .................. 6
2.1.1.3. Numerical studies .................... 9
2.1.2. Compressible Flow Description ................. 11
2.2. Computational Modelling of Turbulence ................ 12
2.2.1. Direct Numerical Solution (DNS) ................ 14
2.2.2. Large-Eddy Simulation (LES) .................. 15
2.2.2.1. Filtering ......................... 16
2.2.2.2. Filtered conservation equations ............ 17
2.2.3. Reynolds Averaged Navier-Stokes (RANS) Equations ..... 18
2.2.3.1. Turbulent-viscosity models ............... 19
2.2.3.2. Reynolds-stress models ................. 23
3. Numerical Analysis 25
3.1. The Square Cylinder Benchmark Case: Description .......... 25
3.1.1. Numerical Grid .......................... 26
3.1.2. Boundary and initial conditions ................. 27
3.1.2.1. Reynolds number analysis ............... 28
IV
Contents
3.1.3. Solver definition .......................... 30
3.1.3.1. Time-step and Courant number ............ 31
3.1.3.2. Solution algorithm ................... 32
3.1.4. Post-process methodology .................... 33
3.1.4.1. Vortex shedding frequency ............... 33
3.1.4.2. Results averaging .................... 36
3.1.4.3. Regions of interest ................... 37
3.1.4.4. Post-processing flowchart ............... 39
3.2. Result discussion for different Hcyl cases ................ 39
3.2.1. Inlet parameter study ...................... 41
3.2.2. Mach number analysis ...................... 42
3.2.3. Flow field and vortex shedding description ........... 43
3.2.4. Result analysis and validation .................. 46
3.2.4.1. Centerline velocity ................... 48
3.2.4.2. Surface pressure coefficient ............... 52
3.2.4.3. Boundary layer development .............. 55
3.2.4.4. Dimensionless wall distance (y+)........... 57
3.2.4.5. Compressibility effects analysis ............ 59
4. Discussion and conclusions 63
4.1. Further research .............................. 64
Appendices 69
A. The Equations of Fluid Motion 69
B. Introduction to turbulence 72
B.1. Statistical description of turbulent flows ................ 73
B.2. Reynolds equations ............................ 74
B.3. Reynolds Stresses ............................. 77
B.4. The energy cascade ............................ 78
B.5. Kolmogrov’s Hypothesis ......................... 81
C. Further Results from the Present Study 83
C.1. Boundary layer development ....................... 83
C.2. Upstream region analysis ......................... 84
C.3. Results for a higher Reynolds number .................. 85
D. Results from Previous ITLR Related Studies 90
V
List of Tables
3.1. Fluid field initialization parameters ................... 27
3.2. Sutherland’s law coefficients [1]..................... 29
3.3. Spectral analysis results for a wide range of cylinder heights ..... 35
3.4. Time-average analysis parameters for one vortex shedding period . . . 36
3.5. Literature results of square-cylinder case mean flow parameters . . . . 47
3.6. Present study square-cylinder cases mean flow parameters ...... 47
3.7.
Maximum, minimum and average dimensionless wall distance
y+
along
the cylinder surface at Re = 20,000 .................. 58
C.1. Cases to study for Hcyl = 0.01 [m]and a variable Reynolds number . . 85
VI
List of Figures
2.1.
Bearman and Obasaju [
2
] experimental results where the bold line is
A/D
= 0 and
Re
= 20
,
000 (a) Vortex shedding frequency versus re-
duced velocity (b) Distribution of mean pressure around an oscillating
square-section cylinder .......................... 7
2.2.
Lyn and Rodi [
3
] comparison of time-averaged velocity (
u
) profiles
(solid line) with phase-averaged velocity (
hui
) profiles: +, phase 5; ,
phase 15. .................................. 8
2.3.
Tian et al. [
4
] square cylinder numerical results (a) Time-averaged
pressure distributions on the surfaces of the square section (b) Mean
streamwise velocity distribution along the center-line ......... 9
2.4.
Younis and Przulj [
5
] square cylinder numerical results (a) Time-
averaged pressure distributions on the surfaces of the square section
(b) Mean streamwise velocity distribution along the center-line . . . 10
2.5. Density changes from M= [0 1] where ρ= 1.225 [kg/m3]...... 12
2.6.
Schematic representation of turbulent motion (left) and time-dependence
of a velocity component at a point (right)[6].............. 16
2.7.
Upper curves: sample velocity field
U
(
x
)and the corresponding filtered
field
U
(
x
)(bold line). Bottom curves: residual field
u0
(
x
)and the
filtered residual field u0(x)(bold line). [7]................ 17
2.8. Example of turbulent spatial scales resolved by modeling approach [8]19
2.9.
Velocity map for SST, SAS, and LES models. Instantaneous and
averaged fields [9]............................. 23
3.1. Schema of the square cylinder benchmark case ............. 25
3.2. Square cylinder structured non-uniform Cartesian grid ........ 26
3.3.
Air thermodynamic properties (a) Density against temperature (b)
Dynamic viscosity against temperature ................. 29
3.4.
Free-stream velocity and Mach number as a function of
Hcyl
at
Re
=
20,000 ................................... 30
3.5. ANSYS CFX Solver algorithm flow chart ................ 32
3.6.
Lift coefficient evolution with envelopes at
Re
= 20
,
000 (a)
Hcyl
=
0
.
0015 [
m
](b)
Hcyl
= 0
.
0020 [
m
](c)
Hcyl
= 0
.
0040 [
m
](d)
Hcyl
=
0.0100 [m]................................. 33
3.7. Spectral analysis for different Hcyl at Re = 20,000 .......... 34
VII
List of Figures
3.8.
Period analysis along steady time steps for
Re
= 20
,
000 and
Hcyl
=
0.0015 [m](a) Period (ts) evolution (b) Strouhal number evolution . 36
3.9. Phase number relationship with the CLphase in radians ....... 37
3.10.
Regions of interest (a) Centerline definition for velocity distribution
analysis (b) Cylinder surface for pressure coefficient study ...... 38
3.11.
Regions of interest (a) Boundary layer thickness (
δ
) and displacement
thickness (
δ1
) (b) Displacement (
δ1
) and momentum (
δ2
) thickness
along the upstream region ........................ 38
3.12.
Regions of interest (a) Plane around the square cylinder (b) Plane
along the square cylinder wake ...................... 39
3.13. Simulation and post-processing flowchart ................ 40
3.14.
Inlet density (
ρ
), dynamic viscosity (
η
), pressure (
P
), temperature
(T) and velocity (U) for different Hcyl cases at Re = 20,000 ..... 41
3.15. M
and
Mmax
in space and time as a function of the cylinder height
[10]..................................... 42
3.16.
Mach field around the square cylinder region for different
Hcyl
at
Phase 5 [10]................................ 43
3.17.
Turbulent kinetic energy (
k
) over the cylinder wake at different shed-
ding phases and
Hcyl
. Here (
)indicates
kmax
, (+) the
kmax
and (
)
the thermal conductivity κmax ...................... 44
3.18.
Non-dimensional turbulent kinetic energy (
k/U 2
), eddy viscosity,
total pressure (
Ptot
), density (
ρ
), temperature (
T
) and Mach fields
and contours over the cylinder wake at Phase 0 and
Hcyl
. Here (
)indicates
Pmax
, (
) the maximum eddy viscosity, (+) the
Tmin
and
() the ρmax ............................... 45
3.19.
Predicted [
5
,
11
,
12
] and measured [
3
,
13
] centerline distributions of
time-averaged velocity (
U
) and normal Reynolds stresses (
R11
and
R22) in streamwise and transverse direction for result validation . . . 49
3.20.
Present study simulations centerline distributions of time-averaged
velocity (
U
) and normal Reynolds stresses (
R11
and
R22
) in streamwise
and transverse direction. ......................... 50
3.21.
Centerline distributions of predicted [
10
] and measured [
13
] time-
averaged periodic and turbulent velocity fluctuations. [10]...... 51
3.22.
Centerline distributions of predicted [
5
] and measured [
14
] phase-
averaged axial and vertical velocities .................. 52
3.23.
Predicted [
5
,
12
] and measured [
15
] mean and r.m.s values of surface
pressure coefficient ............................ 53
3.24.
Present study mean and r.m.s values of surface pressure coefficient
results ................................... 54
VIII
List of Figures
3.25.
Predicted [
5
] and measured [
14
] time-averaged velocity profiles
U/U
over the upper cylinder surface ..................... 55
3.26.
Boundary layer for different
Hcyl
and
Re
= 20 000 (a) Cylinder wall
boundary layer thickness (
δ
) (b) Cylinder wall oundary layer displace-
ment thickness (
δ1
) (c) Wake momentum thickness (
δ2
) (d) Wake
boundary layer displacement thickness (δ1)............... 56
3.27.
Time-averaged dimensionless wall distance
y+
over the square cylinder
surface at Re = 20,000 for different cases of study ........... 58
3.28.
Density (
ρ
) and pressure (
P
) contours and flow streamlines around
the cylinder region at Phase 5 ...................... 59
3.29.
Density (
ρ
) and pressure (
P
) gradients contours and flow stream-
lines around the cylinder region at Phase 5 where
indicates
kmax
....................................... 60
3.30.
Time-averaged density
ρ
and
P
along the upstream region for different
transverse section and Re = 20,000 ................... 62
B.1.
Time history of the axial component of velocity
U1
(
t
)on the centerline
of a turbulent jet. From the experiment of Tong and Warharft (1995) [
7
]
73
B.2.
Energy dissipation law example (a) An automobile subject to a drag
force FD(b) Variation of CDwith Reynolds number [16]....... 79
B.3.
Energy cascade concept (a) Energetic, inertial and dissipation region
in the energy cascade (b) The cascade according to the Kolmogrov
[17] theory ................................ 80
C.1.
Boundary layer development along normal cylinder planes for dif-
ferent
Hcyl
and
Re
= 20
,
000 (a) Vorticity profiles (b) Approximate
separation points ............................. 83
C.2.
Time-averaged density
ρ
and
P
along the upstream region for
Re
=
20,000 ................................... 84
C.3.
Lift coefficient evolution with envelopes for
Hcyl
= 0
.
01 [
m
]at (a)
Re = 20,000 (b) Re = 50,000 (c) Re = 130,000 ............ 85
C.4. Spectral analysis for Hcyl = 0.01 [m]and variable Reynolds ...... 86
C.5. Predicted [5,11,12] and measured [3,13] Centerline distributions of
time-averaged velocity (
U
) and normal Reynolds stresses (
R11
and
R22) in streamwise and transverse directions for result validation . . . 86
C.6.
Centerline distributions of time-averaged velocity (
U
) and normal
Reynolds stresses (
R11
and
R22
) in streamwise and transverse direc-
tions for different Hcyl and Re ..................... 87
C.7.
Predicted [
5
,
12
] and measured [
15
] mean and r.m.s values of surface
pressure coefficient ............................ 88
IX
List of Figures
C.8.
Mean and r.m.s values of surface pressure coefficient for different
Hcyl
and Re ................................... 89
D.1.
Effect of free-stream Mach number on the mean value of drag coefficient
and Strouhal number [10]........................ 91
X
Nomenclature
Latin Symbols
Re - Reynolds number
Re- free-stream Reynolds number (ρUHcyl)
St - Strouhal number (f Hcyl /U)
FN general force vector
CL- square cylinder total lift coefficient
FLN total lift force
CD- square cylinder total drag coefficient
FDN total drag force
Cp- square cylinder pressure coefficient
fHzsquare cylinder vortex shedding frequency
Am cylinder oscillation amplitude
Hcyl m square cylinder height
Ums1free-stream velocity
Lrm length of the recirculation zone
Dm cylinder diameter
Lm three-dimensional cylinder length
x, y, z m Cartesian coordinate system
i, j, k - Cartesian coordinate unit vector
jm y-direction unit vector
km z-direction unit vector
u, v, w ms1velocity components in Cartesian notation
u1, u2, u3ms1velocity components in dimensional notation
n- unit vector normal to the CS
Sm2surface area
mkgmass quantity
.
mkg s1mass flux (U S ρ)
ts time
pPastatic pressure
PtPatotal pressure
TK static temperature
XI
Nomenclature
Vm3volume
vm3kg1specific volume
FgN gravity force
FPN pressure force
Fsurf N surface force
gms2gravity acceleration vector
Qkg m2s2heat
Wkg m2s2work
Ekg m2s2energy
em2s2energy per unit mass
ˆum2s2internal energy per unit mass
ˆ
hm2s2enthalpy per unit mass
hUims1mean of the random variable U
Urms1relative velocity
U
(
x, t
)
ms1Eulerian velocity
ums1velocity fluctuation in U
huiujim2s2Reynolds stresses
U
(
x, t
)
ms1filtered velocity field
u0
(
x, t
)
ms1residual filtered velocity field
km2s2turbulence kinetic energy
aij m2s2anisotropy tensor
bij m2s2normalized anisotropy tensor
lm turbulent motions width
kw- wave number
m2s3rate of production of the turbulent kinetic energy
<ij m2s3pressure-rate-of-strain tensor
Tkij m2s3Reynods-stress flux
ts- number of time-steps
Tvs vortex shedding period
κW·m1·K1thermal conductivity
µT- eddy viscosity
np- vortex shedding phase number
R11 m2s2apparent normal Reynolds stress in the steamwise direction
R11 m2s2apparent normal Reynolds stress in the transverse direction
uτm/s wall friction velocity
y+- dimensionless wall distance
Greeke Symbols
αW/(m2K)heat transfer coefficient
XII
Nomenclature
ρkg m3density
µkg m1s1dynamic viscosity
νms1kinematic viscosity
δm boundary layer thickness
δ1m boundary layer displacement thickness
δ2m boundary layer momentum thickness
δij m Kronecker delta function
σij Nm2surface stress tensor
τij Nm2viscous stress tensor
τs eddy characteristic timescale
εm2s3turbulent energy dissipation
εij m2s3turbulent energy dissipation tensor
σk- Prandtl number
φi- arbitrary variable
τWNm2wall shear stress
Indices
0large scale turbulent motions
ηKolmogorov scale turbulent motions
free-stream condition
Abbrebiations
RANS Reynolds Averaged Navier-Stokes
URAN S Unsteady Reynolds Averaged Navier-Stokes
LES Large-Eddy Simulation
DN S Direct Numerical Simulation
SST Shear Stress Transport
CV Control Volume
CS Control Surface
RMS Root Mean Square
ODE Ordinary Differential Equation
P DF Probability Density Function
CDF Cumulative Distribution Function
CDS Central Difference Scheme
H P C High Performance Computing
SAS Scale Adaptative Simulations
ISA International Standard Atmosphere
FFT Fast Fourier Transform
XIII
1. Introduction
1.1. Motivation
Turbulence and chaos are phenomena present in our everyday that sometimes goes
unnoticed. One can observe it in the clouds or the air moved by a butterfly flapping,
both examples of the large and small scales of turbulence. The beauty of this
phenomena has captivated many curious minds who tried to reveal its secrets along
decades. Unfortunately, its analysis and understanding come along with a big
mathematical and physical background available to few.
One of the main motivations of the author was to obtain a better insight in this
field of study. Despite having a good background in the numerical analysis and
Computational Fluid Dynamics field, understanding the turbulence behavior is still
a challenging task. Therefore, the ITLR research proposal was a perfect opportunity
to get in touch with this field of study.
1.2. Scope of the thesis
The flow around a square cylinder constitutes a canonical configuration to study the
flow around bluff bodies because of its importance in numerous technical applications,
e.g structural response of skyscrapers to aerodynamic forces and the mixing of two or
more fluids. Most of the fundamental experimental work has been completed within
the last century [
2
,
13
15
,
18
] setting the bases for the present computational analysis.
Therefore, different numerical methods of different accuracy and computational costs
such as Unsteady Reynolds-averaged Navier-Stokes (URANS) simulation [
4
,
5
,
10
],
Large Eddy Simulation (LES) [
11
,
19
], and Direct Numerical Simulations (DNS) [
12
]
have been applied.
The current study focuses on solving the two-dimensional square cylinder case
by applying a turbulent-viscosity model. Specifically, it is utilized the URANS
approach with the implementation of the Menter
kω
model also known as Shear
Stress Transport (SST) model. Because of the complexity of turbulent vortex
shedding predictions it is required to obtain a set of representative parameters
for describing the phenomenology. These include global dimensionless quantities
to describe the frequency and strength of the vortex shedding, instantaneous and
mean flow parameters along the wake centerline, and the cylinder surface pressure
1
Introduction 1.3 Contents description
distribution. Once the final results are obtained, these are validated using the data
from cited publications for a final analysis under compressible flow conditions.
The main objective of this thesis is to predict the vortex shedding behind a
two-dimensional square cylinder to evaluate the URANS simulation capabilities.
Additionally, the secondary objectives are listed below:
(i) Gain relevant knowledge about turbulence and its computational analysis.
(ii) Unsteady flow transient analysis with ANSYS CFX & ICEM software.
(iii) Understanding the main features of the square cylinder case flow field.
(iv) Evaluation of the URANS-SST approach performance.
(v)
Assessment of compressibility effects and its coupling with the turbulent phe-
nomenology.
(vi)
Produce results with scientific value, thus defining the steps to follow in future
studies.
1.3. Contents description
This thesis is divided into three main chapters consisting on the theoretical back-
ground, the numerical analysis and lastly the conclusions of the study. First of all,
in the theoretical background a literature review section, that provides a time-line
description about the methodologies implemented on the case of study, is provided.
Afterwards a section which explains different approaches for the computational
modeling of turbulence, focusing on the Reynolds-averaged Navier-Stokes (RANS)
methodology is introduced.
Secondly, the numerical analysis chapter displays the followed methodology and
results of the research performed. In that chapter, the main ingredients for the
numerical analysis such as the mesh, boundary conditions and solver definition are
described. Finally, the results obtained during the study are presented and its main
features are described. Lastly, in the conclusion the most relevant aspects of the
research are summarized.
2
2. Theoretical Background
2.1. Literature Review
The term "turbulence" was introduced in a scientific context by Thompson in 1887
as stated by Schmitt in [
20
]. At the beginning, this term was not adopted by great
authors as Osborne Reynolds or Lord Rayleigh but in the 1920s it became a classical
term. Nowadays, one can find thousands of papers related to the topic. A fast Web
of Science search reveals more than 36,000 papers published between 1991 and 2021,
with 8,719 alone for the year 2015.
It was a century after the first turbulence related studies that Kolmogorov attemp-
ted to predict the properties of flow at very high Reynolds numbers (fully developed
turbulence) giving birth to its very brief third 1941 paper "Dissipation of energy
in locally isotropic turbulence" (Kolmogorov 1941c [
17
]). Although some of the
presented ideas can be criticized as mathematically or physically inconsistent, as
Frisch [
16
] stated, its work has been and remains a major source of inspiration. The
familiarity with the Kolmogorov’s hypothesis is nowadays a must for any researcher
related to the field of study.
Once given an introduction to the research related to turbulence it is now time to
focus on our case of study. The studies related to the prediction of vortex shedding
from smooth cylinders can be divided as in most of the fluid field studies into two
main types, experimental and numerical studies. The flow analysis around a bluff
bodies at high Reynolds numbers has been a problem of interest since the second
part of the 20th century. The experimental research was the one that placed the
first stones for the comprehension of such case until major advances in computation
came at the ends of this century.
Several experimental studies were performed from the 1970s and much has been
written on the subject of vortex-induced oscillation of bluff bodies. B. E. Lee
[
15
] stated that from an engineering point of view the case was interesting for an
economical design of buildings and structures. Thus, it was required for a theoretical
or empirical solution for the problem simplification but another problem was a
coherent scaling of the atmospheric turbulence to a wind tunnel experimental case.
Until this point, little information were available on the effects of turbulence on
vortex shedding from sharp edge bluff body structures, although this was a problem
of considerable practical significance. It is also important to consider the work from
3
Theoretical Background 2.1 Literature Review
Lyn & Rodi [
3
] about the similarity behavior of the phase-averaged profiles in the
shear layer as well as the streamwise growth of the shear layer investigation. Lyn et
al. [
14
] further investigations present an analysis on the flow topology and turbulence
relationship. In fact, the topology of the square and circular cylinders is expected
to be identical, but differences in length and velocity scales provided insight into
the relationship between "coherent" vortex structures and "incoherent" (or "random")
turbulent characteristics.
It was during the 1990s decade when the first numerical studies related to the flow
analysis around bluff bodies were presented. These studies came along with the rapidly
increasing computational capacity and a much more affordable technology. During
these years it was common to use self-developed software for the numerical studies.
However, with the development of the CFD field a lot of new companies devoted to
the software development released their own products. It is true that for the top
level scientific research it is always better to have state-of-the art methodologies
implemented in its own advanced solving software but the commercial software
availability to the general user brought the possibility of modeling the fluid field in an
easier, more efficient way. In 1997 Wissink [
21
] presented a DNS of a 2D setup for a
square cylinder case that showed the behavior of the monopolar, dipolar and tripolar
generated vortices for a
Re
= 10
,
000. The same year Rodi [
19
] presented a LES and
RANS comparison at
Re
= 22
,
000 using the square cylinder case and compared the
numerical results with the ones that he obtain in his previous experimental realization.
In his study, he concludes that the results obtained predicted reasonably well these
complex flows despite the fact that they were not entirely satisfactory. In all RANS
calculations the turbulence fluctuations were severely underpredicted. The deviation
of the results with the experiments were attributed to the insufficient resolution near
the walls, numerical diffusion and insufficient domain extent and number of grid
points in the spanwise direction. These first results, despite not being completely
accurate, were in fact promising and provided the first guidelines for the improvement
of the numerical methodology used. During the coming years, several efforts were
invested on the implementation of different turbulence modeling methodologies such
as DNS, LES, RANS and URANS using various modeling techniques that improved
the correlation of the numerical and experimental results. In order to compare the
numerical results the researchers brought the idea of using a specific flow topology
as a benchmark case. Therefore, the square cylinder case was studied as canonical
configuration for the flow around bluff bodies because it was found that occurrence
of vortex shedding at a sufficiently high Re number arise at a well-defined frequency.
Since Bradshaw [
22
] wrote ’the best modern methods allow almost all flows to
be calculated with higher accuracy than the best-informed guess, which means
that the methods are genuinely useful even if they cannot replace experiments’,
RANS models have improved considerably. The first RANS numerical researches
4
Theoretical Background 2.1 Literature Review
were mainly conducted using turbulent-viscosity models such as the Launder [
23
]
kε
model, the Wilcox [
24
]
kω
and the Mentre’s [
25
] SST model due to their
engineering application relevance. The use of RANS came together with the URANS
methodology, which provided a more illustrative representation of the calculated flow
in exchange of a greater computational cost. Most of the recent research focuses
on the improvement of the RANS models in order to achieve a better agreement
of the results with the ones obtained using LES and DNS. Younis and Przulj [
5
]
presented a computational study using URANS focus on developing a modification
for the
kε
model. The obtained results showed the potential of their approach
because a better correlation with experimental and other more accurate numerical
studies was observed. All the computational advancements and the improvement
of RANS and URANS are pushing their use for solving complex geometries for
engineering applications, since they provide accurate enough solutions for a relatively
low computational cost. These advancements would not have been possible without
the big collective effort from lots of great authors on the turbulence modeling field
of study.
Finally, it should be noted that although lots of advancements were done, turbulence
modeling is a large field and there are still questions to be answered. One of these
questions is how the compressibility affects the fluid in a turbulent flow. There is
some literature related to this topic but the mathematical complexity arises from the
consideration of a variable density leads the turbulence problem to a more complex
approach. Papamoschou and Roshko [
26
] presented an experimental study about the
compressible turbulent shear layer and Dongru Li et al. [
27
] published a numerical
study of compressibility effects in a turbulent mixing layer. The revision of the
related literature shows that nowadays there is still not a compressibility effects study
conducted using the square cylinder case. Thus, there is a gap that still needs to be
filled in the flow analysis around bluff-bodies using the square-cylinder benchmark
case.
2.1.1. Square cylinder case results
In the previous paragraphs it was explained the turbulence related scientific research
that brought the interest for the study of the square cylinder case. The possibil-
ity of implementing different turbulence modeling methodologies for analyzing its
performance raised the interest of using this topology as a benchmark case. In this
section the main experimental and numerical research concerning the square cylinder
problem is summarized. The Reynolds number of interest for the thesis study is
Re = 20,000 because most of the literature studies use similar values.
5
Theoretical Background 2.1 Literature Review
2.1.1.1. Mean-flow parameters
Table 3.5 shows the numerical and experimental results performed by different
studies on the case of the square-cylinder benchmark case using different models
and methodologies. In order to understand the results shown in those studies it is
important to define the mean-flow parameters typically used to describe the turbulent
vortex shedding. The parameters consist on:
(i)
Strouhal number (
St
). Dimensionless parameter used to describe the oscillating
flow mechanisms as a function of the vortex shedding frequency
f
and the
problem parameters such as the cylinder height
Hcyl
and the free-stream velocity
Hcyl.
St =f Hcyl
U
(2.1)
(ii)
The lift (
CL
) and drag (
CD
) coefficients, which express the total lift (
FL
) and
drag (
FD
) force over the square-cylinder. The literature results show the mean
drag coefficient
hCDi
and the Root Mean Square (RMS) of the lift and drag
coefficient (C0
LC0
D). As it is well known,
CD=FD
0.5ρU2
and CL=FL
0.5ρU2
(2.2)
(iii)
The final represented result is the time-averaged length of the recirculation
zone expressed by
hLri/Hcyl
where
hLri
is the mean recirculation zone length.
2.1.1.2. Experimental studies
In the experiment conducted by Lee [
15
], the empirical equipment consisted on a
square prismatic cylinder measuring 165 x 165
mm2
mounted in a low speed wind
tunnel. The tests were conducted on the square cylinder in a uniform flow and in
homogeneous turbulent flows at
Re
= 1
.
76
·
10
5
. The Reynolds number for the flow
in this study is greater than the one studied in this thesis but it is interesting for
analyzing the influence of the
Re
number on the vortex shedding. Their measurements
presented the effects of uniform and turbulent flows on a two-dimensional square
cylinder. It was found that the addition of turbulence to the flow raised the base
pressure and reduced the drag of the body. This result is attributed to the manner in
which the turbulence intensity thickens the shear layers, causing them to be deflected
by the downstream corners of the body and resulting in the downstream movement
of the vortex formation region. Thus, the strength of the vortex shedding is shown
to be reduced as the intensity of the incident turbulence is increased.
The experiment conducted by Bearman and Obasaju [
2
] measured the pressure
fluctuations acting on a stationary square cylinder, with the front face normal to the
flow, and one forced to oscillate transverse to the flow. The main objective was to
6
Theoretical Background 2.1 Literature Review
(a) (b)
Figure 2.1.:
Bearman and Obasaju [
2
] experimental results where the bold line is
A/D
= 0
and
Re
= 20
,
000 (a) Vortex shedding frequency versus reduced velocity (b)
Distribution of mean pressure around an oscillating square-section cylinder
study the vortex-induced oscillation of a bluff body. The experimental arrangement
was performed in a low-speed, closed wind tunnel at nominally atmospheric pressure
with a working section of 0
.
92
m
square and 4
.
9
m
long. In their studies the vortex-
shedding frequency
n
was estimated from the power spectra of pressure fluctuations
recorded at the center of a side face of the square section. Figure 2.1a represents
the shedding frequency of the stationary model
A/D
= 0, where A is the oscillation
amplitude and D is the section dimension which remains constant. There, the reduced
velocity
U/ND
at which
n/N
= 1 (where
N
is the cylinder oscillation frequency)
is equal to the inverse of the stationary-body Strouhal number. From the plot the
reduced velocity value of 7
,
7gives a Strouhal number of 0.13. The mean pressure
distribution around the cylinder was also measured. Figure 2.1b shows the pressure
coefficient distribution along the points
ABCD
, this shows clearly the
pressure recovery due to the detachment of the boundary layer.
Luo et al. [
18
] conducted an experimental research on the effects of incidence and
after-body shape on flow past bluff bodies. The experiment was conducted in a
wind tunnel which dimensions 1 m (W) x 0.6 m (H) x 2.75 m (L) with a turbulence
intensity less than 0
.
5%, an experimental free-stream velocity (
U
= 10
m/s
) and
Re
= 3
.
4
·
10
4
. Most of their study is focused on how the square-cylinder rear shape
modification affects the vortex shedding and the main parameters of the problem.
However, this experimental research is considered for its scientific value and the
amount of results provided that can be correlated with the thesis studies as shown
in Table 3.5.
The last experimental research that is to be presented is the one developed by Lyn
7
Theoretical Background 2.1 Literature Review
Figure 2.2.:
Lyn and Rodi [
3
] comparison of time-averaged velocity (
u
) profiles (solid line)
with phase-averaged velocity (hui) profiles: +, phase 5; , phase 15.
and Rodi [
3
]. Their study consisted on the analysis of flapping shear layer formed
by flow separation from the forward corner of a square cylinder. In their study the
similarity behavior of the phase-averaged profiles in the shear layer as well as the
streamwise growth of the shear layer has been investigated. The turbulent separated
flow around two-dimensional bluff bodies exhibits a self-induced quasi-periodicity
due to vortices being "shed" alternately from either side of the body. The researchers
selected the square cylinder case as a simple, compactly characterized bluff body
where the separation point(s) are fixed and known. A further advantage is the
geometry, a highly favorable pressure gradient just prior to separation results in
an extremely thin separating shear layer; effects on shear layer development due to
initial shear-layer thickness should therefore be negligible.
Measurements were made in a closed water channel with a working cross-section of
56 cm
·
39 cm. The square aluminum cylinder was of diameter
D
= 4
cm
, and length
L
= 39
cm
, resulting in a blockage of 7% and an aspect ratio of 9
.
75. Figure 2.2
shows the deviation of phase-averaged velocity (
hui
) profiles from the time averaged
(
u
) profiles for two selected phases, one during acceleration (phase 5) and one during
deceleration (phase 15). At the upstream section (
x
= 0) the deviations are relatively
small; in contrast, at the downstream section (
x
= 1) the deviation considerably
increases. Deviations were found to be largest in the shear layer, the free-steam side
being relatively undisturbed and the wall-side being inhibited by the solid boundary.
In their experiment, Lyn and Rodi [
3
] present a deep flow phase and shear-layer
region analysis. Some important aspects from the Lyn and Rodi experiment have
been commented but it is required to clarify the great value of their research for the
coming numerical advancements in the bluff-body shear-layer study.
8
Theoretical Background 2.1 Literature Review
(a) (b)
Figure 2.3.:
Tian et al. [
4
] square cylinder numerical results (a) Time-averaged pressure
distributions on the surfaces of the square section (b) Mean streamwise velocity
distribution along the center-line
2.1.1.3. Numerical studies
Nowadays there is a large number of numerical studies related to the flow around
bluff bodies. In this part the literature reviewed focuses on the URANS methodology
but LES and DNS simulation approaches are also included in order to give a better
impression of the results obtained in each case. The first case to be discussed is the
URANS simulation of flow around rectangular cylinders with different aspect ratios
performed by Tian et al. [
4
]. In their study a two-dimensional URANS-SST model is
implemented at
Re
= 21
,
000. The simulations were conducted using the open source
CFD code OpenFOAM with a computational domain of 35H by 20H where
H
is the
square cylinder height. The flow inlet boundary is located at a distance 10H of the
centre of the cylinder and the flow outlet boundary is located 25H downstream. As
it is known, the vortex shedding frequencies are not sensitive to the aspect ratio, and
the ratios calculated in the simulations were in good agreement with published results.
In this study, the time averaged pressure coefficient (
Cp
) distribution shown in Figure
2.3a is in a good agreement with the published experimental data and the numerical
results. On the side-surface (0
.
5
xp
1
.
5) and the back surface (1
.
5
xp
2)
CP
does not show a large variation. The mean streamwise velocity distribution along the
centre-line (
x2
= 0) of the square is shown in Figure 2.3b. In the upstream region the
results show a moreover good agreement with the experimental results from Durao et
al. [
13
]. In the wake region the results reasonably agree with the results of Shimada
and Ishihara [
28
] using a modified
kε
model. Both simulations underestimate the
length of the mean recirculation region (
L
). It should also be noted that the values
of
St
are not sensitive to the aspect ratio since it does not affect to the shedding
frequency.
In 2006 Younis and Przulj [
5
] published a paper about the computation of turbulent
vortex shedding. In this publication they state that the principal feature of the flow
9
Theoretical Background 2.1 Literature Review
(a) (b)
Figure 2.4.:
Younis and Przulj [
5
] square cylinder numerical results (a) Time-averaged
pressure distributions on the surfaces of the square section (b) Mean streamwise
velocity distribution along the center-line
around smooth cylinders, and the primarily cause of the difficulty in the prediction, is
the development of a von Karman vortex street leading to significant fluctuations in
the surface pressures. It is also mentioned that the eddy-viscosity closures tend to fail
to capture the correct magnitude of these fluctuations though there is no consensus
to the underlying causes. In this study, their proposal accounts for the energy
transfer process in the turbulent scales in the context of two-equation eddy-viscosity
closures. It is compared to the results obtained with a URANS methodology using
the well known
kε
turbulence model and a modified version. The simulations
were conducted using a finite volume two-dimensional mesh with a computational
domain of 42H by 24H. The inlet boundary is located at a distance 12H from the
center of the cylinder and the outlet is located 30H downstream. Figure 2.4a shows
that the mean pressure distribution is predicted fairly well by all models. Although
the modified model predicts fairly well the mean drag coefficient, the results for the
mean pressure behind the rear corner C appears to show a faster rate of reduction
than is suggested by the data. Figure 2.4b is a plot of the time averaged streamwise
velocity along the center-line. The size of the recirculation zone downstream of the
cylinder is captured quiet well by the modified model when the grid D2 is used to
obtain a similar blockage ratio as in Lyn’s experiments. This parameter is also well
predicted with the LES method. Younis and Przulj conclude that the proposed
model is robust and economical, being based on an eddy-viscosity closure.
Finally, it is important to mention the valuable numerical studies performed by Cao
et al. [
11
] modeling a tree-dimensional case using the LES methodology and the work
from Trias et al. [
12
] on their tree-dimensional DNS studies on the square-cylinder
case. Both cases provides a valuable source of information and data that would
help to compare the results obtained during the thesis. Table 3.5 shows a list of the
main parameters to be analyzed on the square-cylinder case for both numerical and
10
Theoretical Background 2.1 Literature Review
experimental studies. It is also important to remark that not all the aspects from
the literature have been commented and there are more parameters extracted from
the literature that would be susceptible of analysis during the numerical study part
of the thesis.
2.1.2. Compressible Flow Description
Incompressible flows are those for which
Dρ/Dt
= 0, e.g. the substantial derivative
of the density is zero. One special case is when density is constant. In contrast, a
flow where the density changes in dependence of other state variables, e.g.
P
=
ρRT
is called compressible. Truly incompressible flow, where the density is precisely
constant, do not occur in nature. However, there are a number of aerodynamic
problems that can be modeled as being incompressible without any determinant
loss of accuracy. This problem appear for small Mach numbers e.g.
M <
0
.
3. The
current case of study is one of those cases but this thesis aims to model and analyze
the compressiblity effects to test the capabilities of the URANS methodology.
The inclusion of a changing density
ρ
into the equations of fluid motion makes
its treatment more difficult. For the scope of the thesis, compressible Navier-Stokes
equations are not obtained and the efforts are focused onto understanding its physical
meaning and how is it related to the turbulent effects. Please note ρ=f(x, t).
All real substances are compressible to some greater or lesser extent. By definition
compressibility is the amount by which a substance can be compressed when squeezed
or pressed, thus changing its density. In particular, the density
ρ
of the fluid will
change according to the Eq. (2.3)
ρ
ρ=
1 + γ1
2M2
1/(γ1)
(2.3)
From the diatomic gas assumption,
γ
= 1
.
4and in the Figure 2.5
ρ/ρ
is plotted
as a function of M from zero to sonic flow. For
M <
0
.
32 the value of
ρ
deviates
from
ρ0
less than a 5%, and for all practical purposes the flow can be treated as
incompressible. However, for
M >
0
.
32, the variation in
ρ
is larger than 5% and its
change becomes more pronounced as M increases. The Mach number is defined by
the Eq. (2.4) for an ideal gas as
M=U
c=U
γRT
(2.4)
Therefore, in the present study the maximum
Mach
number obtained in the
compressibility effects analysis has to be
M >
0
.
32 in order to obtain large enough
density changes. It is now understood how the compressibility is related to the
fluid velocity but not its relationship with turbulence. There is still not many
research about this topic and the current study focuses on giving the author a better
11
Theoretical Background 2.2 Computational Modelling of Turbulence
Figure 2.5.: Density changes from M= [0 1] where ρ= 1.225 [kg/m3]
understanding about it. From previous studies it is known that compressibility;
inhibits the growth of the momentum shear layer, and suppresses the turbulence
intensity T u and Reynolds stress level in the shear layer;
has a relatively small effect on turbulent eddies in wall-bounded flows;
plays a crucial role in the stability and mixing of shear layers, producing
order-of-magnitude changes compared with the incompressible case.
Until now, the effects of compressibility has been addressed by means of two-stream
shear layers by Papamoschou and Rosko [
26
] and Barre et al. [
29
]. In their studies
it was found that in compressible flows the turbulent diffusion is inhibited and as a
consequence the growth rate is relatively lower.
2.2. Computational Modelling of Turbulence
The first approach to turbulence from the researchers was mainly theoretical but
the technological advancements from the 19th century brought the possibility to
develop experimental setups for the turbulence analysis. There are overall parameters
such as the time-averaged drag or heat transfer that are relatively easy to measure.
Parameters such as the fluctuating pressure within a flow are almost impossible to
measure at the present time and other can not be made with the required precision.
As a result, numerical methods have an important role to play. However, depending
on what it is analyzed in the flow there are some numerical method requirements
that need to be defined.
Based on the Bardina et al. [
30
] method list, the first approach involves the
use of correlations such as ones that give the friction factor as a function of the
12
Theoretical Background 2.2 Computational Modelling of Turbulence
Reynolds number or the Nusselt as a function of the Reynolds and Prandtl numbers.
This method provides a very useful solution for simple types of flows that can be
characterized by just a few parameters. The second approach consists on using
integral equations derived from the equations of motion by integrating over one
or more coordinates (see Appendix A). Usually, the problem is reduced to one or
more Ordinary Differential Equations (ODE) which can be easily solved. The third
approach is based on equations obtained by decomposing the equations of motion
into mean and fluctuating components as stated by Pope [
7
]. An example are the
Reynolds equations derived in the Appendix B.2, these decomposed equations do
not form closed sets and it is required to use turbulence models. Actually, the
turbulence models are dictated by the nature of the procedure used to obtain the
mean and fluctuating equations. In this approach there is mainly two procedures
called RANS and LES. While RANS averages the equations of motion over time
or over an ensemble of realizations (then called URANS) for representing a time
dependent or steady flow, the LES approach achieves the mean by averaging (or
filtering) over finite volumes in space. LES provides an accurate representation of
the largest motion scales of the flow while approximating or modeling small scale
motions. Finally, the fourth approach is Direct Numerical Solution (DNS) in which
the unsteady Navier-Stokes equations are solved for all motions time and length
scales in a turbulent flow.
Since the thesis is focusing on the application of the URANS model to the study
of the square cylinder the LES and DNS methodology will only be briefly discussed
while focusing on the RANS development. As aforementioned, when the Navier-
Stokes equations are averaged, the result is that the equations are not closed because
of the non-linear convective term. This means that the mean equations contain
non-linear correlation terms involving the unknown fluctuating variables. Thus, one
needs to construct models and approximate these correlations. An example is the
approximation of the Reynolds stresses shown in Appendix B.3 which are required
from a model such as the
kε
,
kω
or the Shear Stress Transport (SST) turbulence
model. The previous example is useful to differentiate the turbulence model and the
variable approximation model. Models should then be:
based on rational principles and con-
cepts of physics, rather than intu-
ition;
constructed from appropriate math-
ematical principles, such as dimen-
sional homogeneity, consistency and
frame invariance;
constrained to yield physically real-
izable behaviour;
widely applicable;
mathematically simple;
built from variables with accessible
boundary conditions;
computationally stable;
rotational invariant.
13
Theoretical Background 2.2 Computational Modelling of Turbulence
2.2.1. Direct Numerical Solution (DNS)
The DNS is the most accurate approach to simulate a turbulent flow since it solves the
Navier-Stokes equations without averaging or approximation other than numerical
dicretizations whose errors can be estimated and controlled. It is also the simplest
approach from the conceptual point of view and the results contain very detailed
information about the flow. In such simulations, all of the motions contained in the
flow are resolved. This can be very useful but it is far more information than any
engineer needs and due to its computational cost DNS is not often used as a design
tool. Because the number of grid points that can be used in a computation is limited
by the processing speed and memory of the machine on which it is carried out, DNS
is typically done for geometrically simple domains.
In order to assure that all of the significant structures of the flow are captured,
the computational domain must be at least as large as the physical domain or the
largest turbulent eddy. For assuring a valid simulation it is necessary to capture
all the kinetic energy dissipation. As it is mentioned in Appendix B.4, the energy
dissipation occurs on the smallest scales due to viscosity effects, so the size of the
grid must be on the order of the Kolmogorof scale,
η
. Usually the resolution is stated
as
kmaxη=π
x1.5(2.5)
The use of DNS can help to learn about the coherent structures that exist in the
flow. This wealth of information can then be used to develop a deeper understanding
of the physics of the flow or to construct a quantitative model, perhaps of RANS
or LES type, which will allow other, similar, flows to be computed at a lower cost,
making this models as a useful engineering design tool. According to Ferzinger et al.
[6], some examples for using DNS are:
(i)
Understanding the process for laminar turbulent transition, as well as the mech-
anisms of turbulence production, energy transfer and dissipation in turbulent
flows;
(ii) Simulation of the production of aerodynamic noise;
(iii) Understanding the effects of compressibility on turbulence;
(iv) Understanding the interaction between combustion and turbulence;
(v) Controlling and reducing drag on a solid surface.
For truly large scale computations on parallel systems, essentially explicit codes
based on CDS or spectral schemes are most often used but in some cases, implicit
methods are used for certain terms in the equations [
6
]. The advances on the High
Performance Computing (HPC) field improved the computational performance in
an exponential range, bringing the possibility to the DNS methodology to solve
complex problems more efficiently. Despite this, it is still expensive to conduct this
14
Theoretical Background 2.2 Computational Modelling of Turbulence
simulations but the development of the quantum computing field could bring the
required advancements for DNS to become a common tool in engineering practices.
2.2.2. Large-Eddy Simulation (LES)
As it has been stated, a Large-Eddy Simulation (LES) represents the larger three-
dimensional unsteady turbulent motions, while the effects of the smaller motions
are modeled. The interest in LES comes when large scale unsteadiness is significant
because the large scale unsteady motions are represented explicitly. In LES, the
Navier-Stokes and scalar equations are filtered (averaged) over space. Thus, LES
are three-dimensional and time-dependent. The resulting equations are from the
structure identical to the URANS equations except that the model for the non-closed
term have a different meaning and form. Pope [
7
] gives a description of the four
conceptual steps in LES.
(i)
Afiltering operation is defined to decompose the velocity
U
(
x, t
)into the sum
of a filtered (or resoled) component
U
(
x, t
)and a residual or sub-grid scale
(SGS) component
u0
(
x, t
). The three-dimensional and time-dependent filtered
velocity field U(x, t)is the one that represents the motion of the large eddies.
(ii)
The equations for the evolution of the filtered velocity field are derived from
the Navier-Stokes equations. The momentum equation is the one containing
the residual-stress tensor (or SGS stress tensor) that arises from the residual
motions.
(iii)
The closure is obtained by modeling the residual-stress tensor, most simply by
an eddy-viscosity model.
(iv)
The model filtered equations are solved numerically for
U
(
x, t
), which provides
an approximation to the large-scale motions of the turbulent flow.
The application of the LES methodologies depend on the problem to be considered
and on the numerical methods used. Pope [
7
] provides a list of example cases where
LES can be applied.
(i) Isotropic turbulence using a pseude-spectral method.
(ii) Isotropic turbulence using a finite-difference mehtod.
(iii) Free shear flow using a uniform rectangular grid.
(iv) Fully developed turbulent channel flow using a non-uniform rectangular grid.
(v) The flow over a bluff body (thesis case) using a structured rectangular grid.
(vi) Flow in a complex geometry using an unstructured grid.
As it is already known, turbulent flows contain a wide range of length and time
scales. The range of eddy sizes that might be found in a flow is shown schematically
on the left hand side of Fig. 2.6. The right-hand side of this figure shows the time
15
Theoretical Background 2.2 Computational Modelling of Turbulence
Figure 2.6.:
Schematic representation of turbulent motion (left) and time-dependence of a
velocity component at a point (right)[6]
history of a typical velocity component at a point in the flow. What this image
enlighten is the fact that LES provides a cost efficient solution for representing the
large scale motions. If a more accurate representation of the small scales is required
then one should point to the use of DNS methods. In computational expense, LES lies
between Reynolds-stresses models and DNS, and its use is defined by the limitations
of teach of these approaches. Although expensive, they are much less costly than
performing a DNS simulation of the same flow. In general, because it preferred
method for flows in which the Reynolds number is too high or the geometry is too
complex for the application of DNS.
2.2.2.1. Filtering
Opposed to the DNS case, in LES the velocity field
U
(
x, t
)does not has to be resolved
on lenghtscales down to the Kolmogorov scale
η
. A low-pass filtering operation is
performed so that the resulting filtered velocity field
U
(
x, t
)can be solved on a
coarser grid. Specifically, the grid spacing
h
is proportional to the specified filter
width . The general filtering operation introduced by Leonard [31] is defined by
U(x, t) = ZG(r, x)U(xr, t)dr (2.6)
satisfying the normalization condition
ZG(r, x)dr = 1 (2.7)
The residual field is defined by
u0(x, t)U(x, t)U(x, t)(2.8)
and the velocity field reads as
16
Theoretical Background 2.2 Computational Modelling of Turbulence
Figure 2.7.:
Upper curves: sample velocity field
U
(
x
)and the corresponding filtered field
U
(
x
)(bold line). Bottom curves: residual field
u0
(
x
)and the filtered residual
field u0(x)(bold line). [7]
U(x, t) = U(x, t) + u0(x, t)(2.9)
It is important to state the difference between the Reynolds decomposition and
the previous formulation. Here, the filtered velocity
U
(
x, t
)is a random field and
in general the filtered residual is not zero,
u06
= 0. Figure 2.7 shows a sample
velocity field
U
(
x
)and the corresponding filtered field
U
(
x
)for a Gaussian filter
with
0
.
35. Here it is evident that
U
(
x
)follows the general trends of
U
(
x
). The
lengthscale fluctuations are removed and appear in the residual field u0(x).
2.2.2.2. Filtered conservation equations
The conservation equations that govern the filtered velocity field
U
(
x, t
)are obtained
by applying the filtering concepts to the Navier-Stokes equations. It is important to
know where these equations come from but due to the scope of the thesis the equation
development is not explained (derivation explained in Pope [
7
]). Considering spatially
uniform filters, the filtered incompressible continuity equation is
∂Ui
∂xi
=∂Ui
∂xi
= 0 (2.10)
leading to
∂u0
i
∂xi
=
∂xi
(UiUi) = 0 (2.11)
The conservative form of the filtered momentum equation is
∂Uj
∂t +UiUj
∂xi
=ν2Uj
∂x2
i1
ρ
∂p
∂xj
(2.12)
17
Theoretical Background 2.2 Computational Modelling of Turbulence
Defining the residual-stress tensor as
τR
ij =UiUjUiUj(2.13)
which is analogous to the Reynolds-stress tensor from Eq. (B.13). With the
substantial derivative based on the filtered velocity is
D
Dt
∂t +U· ∇ (2.14)
the filtered momentum equation is rewritten into the following form.
DUj
Dt =ν2Uj
∂x2
i∂τ r
ij
∂xi1
ρ
∂p
∂xj
(2.15)
The conservation of energy for an isothermal flow is obtained by multiplying Eq.
(2.15) by Uj.
DEf
Dt
∂xi
Uj
2νSij τr
ij p
ρδij
=εfr(2.16)
where εand are defined by
εr2νSijSij (2.17a)
≡ −τr
ijSij (2.17b)
In order to close the equations for the filtered velocity
U
(
x, t
)it is needed a model
for the anisotropic residual stress tensor
τr
ij
. The simplest one is that proposed by
Smagorinsky [32].
2.2.3. Reynolds Averaged Navier-Stokes (RANS) Equations
The Reynolds-averaged Navier–Stokes equations (or RANS equations) are time-
averaged equations of motion for fluid flow. The idea behind the equations is
Reynolds decomposition, whereby an instantaneous quantity is decomposed into
its time-averaged and fluctuating quantities. The RANS methodology consists of
solving the Reynolds equations (described in Appendix B.2) to determine the mean
velocity field
hU
(
x, t
)
i
. In the first approaches, the Reynolds stresses are obtained
from a turbulent-viscosity model. The turbulent viscosity can be obtained from an
algebraic relation (such as the mixing-length model) or it can be obtained from
turbulence quantities such as kor
ε
for which modelled transport equations are
solved. In the Reynolds-stress models, modelled transport equations are solved for
the Reynolds stresses
huiuji
and for the dissipation
ε
(or for another quantity, e.g.,
ω
, that provides a length or time scale of the turbulence). Then, Reynolds-stress
models do not require the turbulent-viscosity hypothesis eliminating one of the major
18
Theoretical Background 2.2 Computational Modelling of Turbulence
Figure 2.8.: Example of turbulent spatial scales resolved by modeling approach [8]
assumptions of other turbulence models.
In RANS, the mean flow defined by the time-average is steady. In Unsteady
Reynolds Averaged Navier-Stokes (URANS) equations the averaging removes all
turbulent (random) eddies. Wyngaard [
33
] reminds us ”that the ensemble-averaged
field is unlikely to exist in any realization of a turbulent flow, even for an instant.” If
the average is over all time, then the resulting equations are the traditional steady
RANS equations, the mean flow defined by the average is steady. Figure 2.8 shows a
visual representation of how each of the described methods represent the turbulent
flow over a bluff body. While RANS averages all the turbulent flow features over
time, the URANS methodology allows to visualize this feature in exchange of a
greater computational cost. As stated by Hart [
8
] Reynolds-averaged methods usually
struggle with the simulation of bluff bodies subject to massive separations but they
are economical. Although DNS and refined LES simulations are impressive in the
flow details they produce, and typically viewed as the only method by which to
accurately simulate such flow, day to day use of these methods is beyond the majority
of academia and industry. Instead the majority of users strike a balance between the
accuracy and economy of the solution, hence the continuing popularity of URANS.
2.2.3.1. Turbulent-viscosity models
Turbulent-viscosity models are based on the turbulent-viscosity hypothesis which, as
stated by Pope [
7
], can be viewed in two parts. First, there is the assumption that
at each point and time the Reynolds-stress anisotropy (Eq. (B.26)) is determined
by the mean velocity gradients
hUii/∂xj
. Second, there is the assumption that the
relationship between hUii/∂xjis
huiuji − 2
3ij =νT
hUii
∂xj
hUji
∂xi
(2.18)
or, equivalently,
aij =2νTSij (2.19)
where
Sij
is the rate-of-strain tensor. The previous relationship is analogous to
the relation for the viscous stress in a Newtonian fluid:
19
Theoretical Background 2.2 Computational Modelling of Turbulence
(τij +P δij)=2νSij (2.20)
The turbulent-viscosity models are mainly based on one-equation and two-equation
models. The algebraic models such as the Uniform turbulent viscosity, the mixing-
length and the turbulent-kinetic-energy models form part of these first group. All of
them are interesting for the understanding of how a model is applied in the RANS
methodology but for the scope of the thesis the research is going to focus on the
second group of two-equation models.
A. The kεmodel
The
kε
model belongs to the class of two-equation turbulence models. Here, the
transport equations are solved for two turbulence quantities. Pope [
7
] stated that
the
kε
model was the most widely used turbulence model and was incorporated
in most commercial CFD codes. Jones and Launder [
34
] are appropriately credited
with developing the standard
kε
model, with Launder and Sharma [
35
] providing
improved values of the model constants. Focusing on the square cylinder case, the
kε
model was used by Bosch and Rodi [
36
] comparing it with a modification
suggested by Kato and Launder [
37
]. There, the standard
kε
model was found
to severely underpredict the strength of the shedding motion, mainly because of
excessive production of turbulent kinetic energy in the stagnation region in front of
the cylinder. The modification of the
kε
model proposed by Kato and Launder
[
37
] avoids this problem. Nevertheless, the
kε
model showing a good prediction
behavior on the regions far away from the walls.
In addition to the turbulent viscosity hypothesis, the
kε
model consists of a
model transport equation for
k
and the model transport equation for
ε
and the
specification of the turbulent viscosity as
νT=Cµk2(2.21)
where
Cµ
= 0
.
09 in one of the model constants. The model transport equation of
k
consists of the turbulent-kinetic-energy model transport equation
Dk
Dt =∇ ·
νT
σkk
+ε(2.22)
Here the constant
σk
is usually considered as
σk
= 1. The model transport equation
for the energy dissipation εwhich is mainly empirical
Dt =∇ ·
νT
σεε
+Cε1
℘ε
kCε2
ε2
k(2.23)
20
Theoretical Background 2.2 Computational Modelling of Turbulence
The standard values from the Launder and Sharma [35] are
Cµ= 0.09, Cε1= 1.44, Cε2= 1.92, σk= 1.0, σε= 1.3(2.24)
Recalling that
D
Dt
∂t +hUi·∇ (2.25)
the kand εEq. (2.22 -2.27) model transport equations are written as
∂k
∂t +hUi · k
∂xi
=∇ ·
νT
σkk
+ε(2.26)
∂ε
∂t +hUi · ∂ε
∂xi
=∇ ·
νT
σεε
+Cε1
℘ε
kCε2
ε2
k(2.27)
where is the rate of production of the turbulent kinetic energy:
=−huiujihUji
∂xi
(2.28)
Additionally, as stated by Younis and Abrishamchi [
38
] after their first numerical
research on the square cylinder case, the
kε
model fails on capturing the main flow
features with vortex shedding. It underestimates the magnitude of the fluctuations
on the pressure field resulting in the underprediction of the lift and drag coefficients.
From their previous research, Younis and Przulj [
5
] have argued that "this defect
arises for the inability of this model to account for the interactions of the large-scale,
organized mean-flow unsteadiness due to vortex shedding and the small scale random
motions that characterize turbulence".
B. The kωmodel
According to Pope [
7
], the
kω
was one of the most widely used two-equation
model. It was developed by Wilcox and other researches (see Wilcox [
24
]). In this
model the expressions for
νT
(Eq. (2.21)) and the
k
equation are the same as those
in the
kε
model. As described in detail by Wilcox [
24
], the
kω
model is superior
for boundary-layer flows in both treatment of the viscous near-wall region, and in its
accounting for the effects of streamwise pressure gradients. However, the treatment
of non-turbulent free-stream boundaries is difficult and a non-phisical boundary
condition on
ω
is required. The model equation for
k
is considered to be Eq. (2.26).
For ωthe following transport equation is obtained
Dt =∇ ·
νT
σωω
+Cω1
℘ω
kCω2ω2+2νT
σωkω· ∇k(2.29)
21
Theoretical Background 2.2 Computational Modelling of Turbulence
C. Shear Stress Transport (SST) model
Menter [
25
] proposed a two-equation model designed to yield the best behaviour of
the
kε
and
kω
models named as Shear Stress Transport (SST) model. The
idea behind the SST model is to retain the robust and accurate formulation of the
Wilcox
kω
model in the near wall region, and to take advantage of the freestream
independence of the
kε
model in the outer part of the boundary layer. To achieve
this, the
kε
model is transformed into a
kω
formulation. The original model is
then multiplied by a function
F1
and the transformed model by a function (1
F1
),
and both are added together. The function
F1
will be designed to be one in the near
wall region (activating the original model) and zero away from the surface.
Transformed kεmodel:
Dk
Dt =∇ ·
νT
σ0
kk
+ω(2.30)
Dt =∇ ·
νT
σ0
ωω
+C0
ω1
℘ω
kC0
ω2ω2+2νT
σ0
ωkω· ∇k(2.31)
Original kωmodel:
Dk
Dt =∇ ·
νT
σ00
kk
+ω(2.32)
Dt =∇ ·
νT
σ00
ωω
+C00
ω1
℘ω
kC00
ω2ω2(2.33)
Then, the modified energy dissipation Eq. (2.31) and the turbulence energy Eq.
(2.30) from the
kε
model are multiplied by
F1
and Eq. (2.32) and (2.33) from the
kω
model are multiplied by (1
F1
). Finally, the corresponding equations of each
set are added together to give the new model:
Dk
Dt =∇ ·
νT
σkk
+ω(2.34)
Dt =∇ ·
νT
σωω
+Cω1
℘ω
kCω2ω2+ (1 F1)2νT
σωkω· ∇k(2.35)
Let
φ1
represent any constant in the original
kω
model (
σ00
k, σ00
ω
,
C00
ωi
, ...),
φ2
any
constant in the transformed
kε
model (
σ0
k, σ00
ω
,
C0
ωi
, ...) and
φ
the corresponding
constant of the new model (σk, σω,Cωi, ...), then the relation between them is:
φ=F1φ1+ (1 F1)φ2(2.36)
Menter [
25
] contains the original description of the Shear Stress Transport (SST)
22
Theoretical Background 2.2 Computational Modelling of Turbulence
Figure 2.9.:
Velocity map for SST, SAS, and LES models. Instantaneous and averaged
fields [9]
method. For the uniformity of the thesis the nomenclature and formulation of the
equations have been adapted. Maliska [
9
] applied the SST model using an URANS
approach to a three-dimensional mounted square cylinder case for comparing the
results with LES and Scale Adaptative Simulations (SAS). The study presented
good results when averaged quantities are compared. However, as expected, the
SST model is not able to capture some important contributions of the turbulence
structures. On the other hand, the computational cost for SST was almost three
times lower than for the LES simulations. Figure 2.9 shows the main differences
when representing the flow using the SST, SAS and LES methodologies.
2.2.3.2. Reynolds-stress models
The Reynolds-stress models solve the transport equations for the individual Reynolds
stresses
huiuji
and the energy dissipation
ε
providing a length and time scale of
the turbulent flow. In this models the turbulent viscosity hypothesis is not needed
anymore, avoiding one of the major assumptions of other models. According to Pope
[7] the Reynolds stresses are expressed as
D
Dt huiuji+
∂xk
Tkij =ij +<ij εij (2.37)
where ij is the production tensor of the Reynolds stresses, expressed as
ij =−huiukihUji
∂xk− hujukihUii
∂xk
(2.38)
εij is the dissipation tensor
εij 2ν*∂ui
∂xk
∂uj
∂xk+(2.39)
23
Theoretical Background 2.2 Computational Modelling of Turbulence
the pressure-rate-of-strain tensor <ij is
<ij *p0
ρ
∂ui
∂xk
+∂uj
∂xk
+(2.40)
and the Reynolds-stress flux Tkij is
Tkij =T(u)
kij +T(p)
kij +T(ν)
kij (2.41)
where
T(u)
kij ≡ huiujuki(2.42a)
T(p)
kij 1
ρhuip0iδjk +1
ρhujp0iδij (2.42b)
T(ν)
kij νhuiuji
∂xk
(2.42c)
In the Reynolds-stress model of Eq. (2.37) the ’knowns’ are
hUi
,
hpi
,
huiuji
.
Thus, the mean-flow convection
Dhuiuji/Dt
and the production tensor
ij
from Eq.
(2.38) are in closed form. However, it requires a model for the dissipation tensor
εij
, the pressure-rate-of-strain tensor
<ij
and the Reynolds-stress flux
Tkij
. Special
attention is required when modeling the pressure-rate-of-strain tensor
<ij
. There
is a vast literature related to Reynolds-stress models where
<ij
is modeled as a
local function of
huiuji
,
ε
and
hUii/∂xj
. Pope [
7
] states that most Reynolds-stress
models there is no dependence with the Reynolds number assuming that the terms
modeled are independent of the Reynolds number. However, in DNS simulations
there can be effects due to the Reynolds number. Within the scope of the thesis the
Reynolds-stress models are not described in this section but yet they are named in
the following list:
(i) Return-to-isotropy models
i Rotta’s model
ii Nonlinear return-to-isotropy
(ii) Pressure-rate-of-strain models
i The basic model (LRR-IP)
ii Others
In comparison with the
kε
model, Reynolds-stress models are more costly and
difficult to implement because in general there are seven turbulence equations to
be solved instead of two (for
k
and
ε
). Nonetheless, especially for complex flows,
Reynold-stress models have been demonstrated to be superior to two-equation models.
Pope [
7
] notes that the CPU time for a Reynolds-stress model calculation can be
more than for a kεby a factor of two.
24
3. Numerical Analysis
3.1. The Square Cylinder Benchmark Case:
Description
Previous studies have already stated the relevance of the square cylinder case in
the prediction of the turbulence behavior around bluff bodies. The current study
is preceded by the results obtained by Younis and Przulj [
5
] and further research
developed in the ITLR department of the University of Stuttgart by J. Richter [
10
].
As it has been explained in Section 2.1.1.3, the model implemented by Younis and
Przulj [
5
] followed a URANS methodology using a
kε
and a modification of itself.
For the J. Richter et al. [
10
] analysis, the turbulence viscosity model used was the
Shear Stress Transport model. While both studies presented remarkable results the
one that used the SST model displays a better agreement with previous experimental
and numerical results. It has to be pointed out that both studies used the same
computational domain for an incompressible two-dimensional case with
Re
= 20
,
000.
In contrast with the aforementioned studies, the present research aims to analyze
how compressibility effects can affect the flow compared with the incompressible
case.
y
x
24Hcyl Hcyl
12Hcyl 30Hcyl
U
O= (0,0)
Figure 3.1.: Schema of the square cylinder benchmark case
25
Numerical Analysis 3.1 The Square Cylinder Benchmark Case: Description
The case of study has been approached using the ANSYS CFX 20.2 commercial
software using a finite volume approach for the definition of the mesh and solution
of the govern equations. It mainly consisted of a two-dimensional region as shown in
the Figure 3.1 where the upper and lower boundaries are solid and the left and right
correspond to the inlet and the outlet of the duct. The total dimensions LxH are
(42x24)
Hcyl
where the cylinder lays its center at (12x12)
Hcyl
. This provided setup
avoids the influence of the boundaries over the cylinder and the vortex structures
generated downstream. The setup performance was verified by Younis and Przulj [
5
]
since the obtained results follow the trends from the experimental procedures.
3.1.1. Numerical Grid
One of the first steps is to generate the mesh. The software used for generating
the mesh is ANSYS ICEM. The simulations to be performed aim to solve a two-
dimensional case but the mesh was defined as three-dimensional because ANSYS
CFX can only read meshes with associated volume elements. For this reason, the
three-dimensional mesh was defined with only one volume element along the z-axis.
In order to develop various meshes efficiently the mesh generation was paramet-
erized using the cylinder as it is displayed in Figure 3.1. With this method it was
possible to perform studies over different cases in an easier way. The mesh dimensions
were arrived at as a result of the test reported by Younis and Przulj [
5
] by quantifying
the numerical uncertainty and how the mesh affects the results due to blockage
effects.
Figure 3.2.: Square cylinder structured non-uniform Cartesian grid
26
Numerical Analysis 3.1 The Square Cylinder Benchmark Case: Description
Figure 3.2 shows the numerical grid implemented in the present study. It consists
in a total of 139x122 cells non-uniformly distributed and the nodes are placed using
a cell-centered approach. In order to have a better accuracy near the cylinder region
with 24 cells in contact with each side with a normalized distance from the cell center
to the wall of
nc/H
= 0
.
014. The grid lines were expanded away from the cylinder
with an expansion ratio of 7.5% in each direction. Younis and Przulj [
5
] obtained
in their studies a blockage ratio produced by the solution domain of
Bf
= 4
.
17%.
This is approximately equal to the values obtained in the experiments of Lee [
15
]
and Bearmand and Obasaju [
2
] but is smaller than in the experiments of Lyn and
Rodi [3].
3.1.2. Boundary and initial conditions
For the domain initialization air is selected as the fluid for this study due to its
wider applicability to engineering interest problems. The air itself is a composition
of approximately a 78% of Nitrogen, 28
.
9% Oxygen and the 1
.
1% left are other gases
such as Argon and Carbon Dioxide. In the study it is assumed that the air is a
diatomic ideal gas, which still provides an accurate description of its thermodynamic
properties. In most of the aerospace applications the height above sea level is a key
factor for defining the air properties but in this case it is set to have approximately
sea level conditions. Therefore, the fluid domain is considered to have a
T
= 293
.
15
K
and an initial horizontal velocity of 1
m/s
. The main domain initialization parameters
are shown in the Table 3.1.
Table 3.1.: Fluid field initialization parameters
Initial values u[m/s]v[m/s]w[m/s]Ps[bar]T[K]Tu
Magnitude 1 0 0 1 293.15 5%
For the numerical analysis and development of the case of study it is necessary
to establish the meaning of boundary conditions. Those conditions are the ones
applied to the nodes that draw the boundaries of the domain. When solving ordinary
or partial differential equations in the presence of a boundary, there needs to be a
boundary condition on the solution. Dirichlet boundary conditions are a specification
of the value that the solution takes itself on the boundaries of the domain. This
type of boundary condition is also called a fixed boundary condition. In the present
study the conditions are applied by setting an arbitrary variable
φ
with a prescribed
value at the boundary nodes.
φ=V al (3.1)
When studying the movement of fluids it is often necessary to apply the no-slip
27
Numerical Analysis 3.1 The Square Cylinder Benchmark Case: Description
boundary condition. It tells us that the fluid velocity at all fluid–solid boundaries is
equal to that of the solid boundary:
φ=v;V al =vwall ;v=vwall (3.2)
The use of the no-slip condition illustrates well the use of scientific models and
idealizations but more importantly, that the condition gives us a realistic macroscopic
approach to the model. On the other hand, the Neuman condition when imposed
on an ordinary or a partial differential equation specifies the derivative values of a
solution over the boundary domain:
dn =V al (3.3)
One possible application is to describe the heat flux over a surface. For example,
if an adiabatic boundary is desired it would be necessary to set this derivative to
zero. The used boundary conditions are described in the following points.
Inlet: Subsonic flow regime with Dirichlet condition for setting the velocity
field as (
u, v, w
)=(
U,
0
,
0). The inlet turbulence modeling parameters are
defined by the
Tu
= 0
.
02 and eddy viscosity ratio
ηt
= 88. The static
temperature is defined as T= 298.15 k
Outlet: Subsonic flow regime with Neuman condition
∂φ/∂x
= 0 for defining
the boundary as an outlet and
∂v/∂y
= 0 for setting a zero vertical velocity.
The relative pressure is set as Pr= 1 bar.
Cylinder: Adiabatic smooth wall with no-slip boundary condition.
Walls: Symmetry condition.
Younis and Przulj [
5
] proved that using the grid shown in Figure 3.2 the mean-
flow parameters such as the Strouhal number and the lift and drag coefficients are
practically insensitive to the levels of turbulence intensity in the incident stream as
long as 0
< Tu<
0
.
02. However, this can be only affirmed for the incompressible
case and its validity needs to be reviewed under compressible flow conditions.
3.1.2.1. Reynolds number analysis
One of the main parts for defining the inlet boundary conditions and the mesh sizes
comes from the Reynolds number analysis. It is well known that the turbulence
effects grow as the Reynolds number increases. In order to keep a compromise
between cost and accuracy the selection of a reasonable Reynolds number is required.
28
Numerical Analysis 3.1 The Square Cylinder Benchmark Case: Description
(a) (b)
Figure 3.3.:
Air thermodynamic properties (a) Density against temperature (b) Dynamic
viscosity against temperature
Thus, in this research the Reynolds has been set to a value of
Re
= 20
,
000. Moreover,
most of the literature used for comparing the results used the same or very similar
values of the Reynolds number. The Reynolds number for the case of study is defined
by the free-stream velocity, the cylinder height and the fluid of study density and
viscosity conditions as
Re=ρUHcyl
µ
(3.4)
By fixing
Re
and calculating
ρ
and
µ
it is possible to define the free-stream
velocity of study as a function of the cylinder height. This result is essential for
defining the inlet boundary condition for each
Hcyl
of interest. In order to obtain
U
=
f
(
Hcyl
)it has been analyzed how the Reynolds number is affected by the
temperature variations by relating the dynamic viscosity to the temperature using
the Shuterland’s law [1] which reads as
µ=µref
T
Tref
Tref +S
T+S(3.5)
The Sutherland’s law coefficients for the fluid of study, which is the air, are
expressed in Table 3.2.
Table 3.2.: Sutherland’s law coefficients [1]
Gas µref [kg/ms]Tref [K]S[K]
Air 1,716 ·105273,15 110,4
Figure 3.3a shows how the density decreases with increasing temperature and how
the dynamic viscosity increases. Using the inlet boundary conditions the temperature
29
Numerical Analysis 3.1 The Square Cylinder Benchmark Case: Description
Figure 3.4.: Free-stream velocity and Mach number as a function of Hcyl at Re = 20,000
is fixed to 298
,
15
K
giving a dynamic viscosity of 1
,
849
·
10
5kg/
(
ms
)and a density
of 1
,
1840
kg/m3
. Setting the air properties, the free-stream velocity can be estimated
as a function of the cylinder height, providing a better way to estimate at which
velocity the compressibility effects are getting visible. In particular, the density of the
fluid will change according to Eq. (2.3). Recalling what it has been aforementioned
in the Section 2.1.2, the flow is considered compressible when the density changes
are greater than a 5%. This mainly occurs when M>0.32.
Including the Mach number definition from Eq. (2.4) into Eq. (3.4) one obtains
M
=
f
(
Hcyl
). Figure 3.4 shows this relationship where the horizontal line denotes
M
= 0
.
32 which represent the limit where compressibility effects arise. Here it is
seen that, in order to study compressibility effects, the cylinder height should be
lower than 0
.
0028 [m]. Nonetheless, it is also important to include in the study values
from the incompressible region since most of the numerical and experimental studies
were developed under this flow field conditions. Thus, the cylinder heights of interest
are defined from the results shown in Figure 3.4 as
Hcyl ={1,1.5,2,2.5,3,3.5,4,10}[mm](3.6)
It has to be taken into account that the case of study is not going to be fully
analyzed for each cylinder height presented. Therefore, after a vortex shedding
and fluid field analysis the most representative
Hcyl
will be selected for the final
presentation of the results.
3.1.3. Solver definition
Once the cylinder height is defined it is possible to define the mesh for each case
of study and also the boundary conditions to be applied in the solver definition.
The simulations are performed using the ANSYS CFX 20.2 software. It uses a
cell-centered finite volume approach on a non-uniform structured three-dimensional
30
Numerical Analysis 3.1 The Square Cylinder Benchmark Case: Description
grid in order to solve the Unsteady Reynolds Averaged Navier-Stokes equations. As
it is aforementioned, the turbulence model selected for the simulation is the Mentre
SST model already explained in Section 2.2.3.1.
The software solves the fluid field by using the equations of fluid motion presented
in Appendix A. Introducing the average and fluctuating components one obtains the
modified RANS equations shown in Appendix B.2. In this case, since the objective
is to study the transient behavior where the averaged component is given by
hUi=1
tZt+∆t
tU dt (3.7)
where
t
is a time scale that is large relative to the turbulent fluctuations, but small
relative to the time scale for which the equations are solved. The averaging shown in
Eq. (3.7) gives the ensable-average RANS equations also called URANS equations.
3.1.3.1. Time-step and Courant number
The time scale
t
presented in Eq. (3.7) is one of the most important parameters
to be defined. Its definition comes from a compromise in between accuracy and
computational cost. A too large value of
t
will not produce valid results and at
the same time a too small value will increase the solution time and therefore, the
computational costs.
The criteria used for defining
t
is the Courant-Friedrichs-Lewy (CFL) condition.
The principle behind the condition relies in the fact that
t
must be less than the
time for the fluid field perturbation to travel to an adjacent grid point. The CFL
condition reads for the x-axis as
C=ut
xCmax (3.8)
where C is called Courant number and
x
is the smallest length interval in the
domain. The value of
Cmax
changes with the method used to solve the discretised
equations, especially depending on whether the method is explicit or implicit. As an
implicit code, ANSYS CFX does not require the Courant number to be small for
stability. However, in a transient calculation one may need the Courant number to
be small in order to accurately resolve the transient details. Thus, the
Cmax
value is
set to be 1. Since the mesh is already defined, the smallest length
x
is easily found
to be
x= 0.0078Hcyl (3.9)
Including the previous relationship into Eq. (3.8) the time-step length is finally
defined as
t=Cmaxx
U
= 0.0078CmaxHcyl
U
(3.10)
31
Numerical Analysis 3.1 The Square Cylinder Benchmark Case: Description
3.1.3.2. Solution algorithm
ANSYS CFX uses a coupled solver, which solves the flow field equations for the
velocity
U
and pressure
P
fields as a single system. The solution approach uses
a fully implicit discretization of the equations at any given time-step. The flow
chart shown in Figure 3.5 illustrates the general field solution process used in the
CFX-solver. The solution of each set of field equations consists of two numerical
intensive operations. For each time-step:
1.
Coefficient generation where the nonlinear equations are linearized and as-
sembled into the solution matrix.
2.
Equation solution where the linear equations are solved using an Algebraic
Multigrid method.
START
Initialize Solution fields and Boudary Condtions
Input ANSYS ICEM Mesh
Solve mesh displacements
Solve Wallscale
Solve Hydrodynamic System
Solve Volume Fractions
Solve Additional Variables
Solve Energy
Solve Turbulence
Solve Mass Fractions
No
Yes
Tansient
No
Yes
Convergece
criteria / Max
Iteration Satisfied
Advance in
False Time
Solve Full Coupled Partivles
Solve One Way Coupled Particles
STOP
No
Yes Coefficient Loop
Criteria Satisfied
Iteration within the
Timestep
Yes
No
Maximum Time
Reached?
Advance in
Time
Figure 3.5.: ANSYS CFX Solver algorithm flow chart
32
Numerical Analysis 3.1 The Square Cylinder Benchmark Case: Description
(a) (b)
(c) (d)
Figure 3.6.:
Lift coefficient evolution with envelopes at
Re
= 20
,
000 (a)
Hcyl
= 0
.
0015 [
m
]
(b) Hcyl = 0.0020 [m](c) Hcyl = 0.0040 [m](d) Hcyl = 0.0100 [m]
3.1.4. Post-process methodology
A development of a suitable post-processing methodology is essential for any flow
field simulation. In the present study each case has to be computed two times. First
of all, an initial simulation is performed for assessing whether the steady state is
reached or not. If achieved, the first results are analyzed for defining the parameters
for the second simulation. This methodology allows to reduce the amount of data
to be stored for each simulation since saving the flow field at each time step is not
an option. Once the final results are obtained they are stored and analyzed using
the CFX-post tool. This software has very useful tools and capabilities for a basic
flow field analysis but for the aim of the study most of the data had to be exported
into text format files in order to perform a deeper analysis using self-developed data
treatment Matlab codes.
3.1.4.1. Vortex shedding frequency
During the definition of the solver it have been set different variable monitoring in
order to have a quick analysis of the results. Two of the mean parameters to monitor
during the transient simulation is the lift and drag coefficient of the square cylinder.
Observing their evolution during each solving time step tells when the results stabilize,
33
Numerical Analysis 3.1 The Square Cylinder Benchmark Case: Description
giving the range where the steady state of the simulation is reached. During the
steady state
CL
oscillates due to the effect of the vortex shedding. Therefore, by
analyzing the lift it is possible to obtain the vortex shedding frequency and the time
steps to be analyzed in the second simulation.
Figure 3.6 shows the evolution of
CL
for different cases where the upper and lower
wave envelopes are shown. Figure 3.6a shows the evolution of
CL
for
Hcyl
= 0
.
0015 [
m
].
Here it is observed that this coefficient oscillate with at least two different frequencies,
a smaller one defined by the envelopes and a greater one that can be extracted from
the data comprehended inside the envelopes. Comparing these results with the ones
displayed in Figure 3.6d for
Hcyl
= 0
.
01 [
m
], it is seen that the
CL
only oscillate with
one frequency and the envelope has a constant value when the steady state is reached.
The behavior for
Hcyl
= 0
.
0015 [
m
]is not the expected one but the explanation for
this phenomena may be related to how the compressibility affects the results.
In Figure 3.7 a spectral analysis of the
CL
evolution is shown for various cylinder
heights. The analysis was performed by using the Fast Fourier Transform (FFT)
methodology. In this plot it is observed that there is only one predominant resonance
frequency (
f0
) for the higher
Hcyl
but when its height is decreased the spectral
analysis starts showing smaller peaks at both sides of the main frequency. Here, the
aforementioned difference between the
Hcyl
= 0
.
0015 [
m
]case and the other ones is
obvious since the secondary frequencies have a greater value.
Another important result that can be extracted from this data is the vortex
shedding period (
Tv
). With this it is possible to know the initial (
ts0
) and final
(
ts1
) time-steps to exactly analyze one vortex shedding period during the second
simulation. Knowing this value and the length of the time step in seconds it is
possible to reach further results such as the Strouhal Number (see Eq. (2.1)). Table
3.3 summarizes the results obtained from the frequency analysis and also includes the
inlet velocity and Mach number for different cases. The
St
number results displayed
were computed using the resonance frequency for each case but is should be taken
into account that its value could not be constant due to the effect of secondary
oscillation frequencies.
Figure 3.7.: Spectral analysis for different Hcyl at Re = 20,000
34