Content uploaded by Miquel Altadill

Author content

All content in this area was uploaded by Miquel Altadill on Oct 18, 2021

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

k−ω

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

k−ω·

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

k−ω

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

k−ω·

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

Nomenclature

Latin Symbols

Re - Reynolds number

Re∞- free-stream Reynolds number (ρ∞U∞Hcyl/µ∞)

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

U∞ms−1free-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 ms−1velocity components in Cartesian notation

u1, u2, u3ms−1velocity components in dimensional notation

n- unit vector normal to the CS

Sm2surface area

mkgmass quantity

.

mkg s−1mass ﬂux (U S ρ)

ts time

pPastatic pressure

PtPatotal pressure

TK static temperature

XI

Nomenclature

Vm3volume

vm3kg−1speciﬁc volume

FgN gravity force

FPN pressure force

Fsurf N surface force

gms−2gravity acceleration vector

Qkg m2s−2heat

Wkg m2s−2work

Ekg m2s−2energy

em2s−2energy per unit mass

ˆum2s−2internal energy per unit mass

ˆ

hm2s−2enthalpy per unit mass

hUims−1mean of the random variable U

Urms−1relative velocity

U

(

x, t

)

ms−1Eulerian velocity

ums−1velocity ﬂuctuation in U

huiujim2s−2Reynolds stresses

U

(

x, t

)

ms−1ﬁltered velocity ﬁeld

u0

(

x, t

)

ms−1residual ﬁltered velocity ﬁeld

km2s−2turbulence kinetic energy

aij m2s−2anisotropy tensor

bij m2s−2normalized anisotropy tensor

lm turbulent motions width

kw- wave number

℘m2s−3rate of production of the turbulent kinetic energy

<ij m2s−3pressure-rate-of-strain tensor

Tkij m2s−3Reynods-stress ﬂux

ts- number of time-steps

Tvs vortex shedding period

κW·m−1·K1thermal conductivity

µT- eddy viscosity

np- vortex shedding phase number

R11 m2s−2apparent normal Reynolds stress in the steamwise direction

R11 m2s−2apparent 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 m−3density

µkg m−1s−1dynamic viscosity

νms−1kinematic viscosity

δm boundary layer thickness

δ1m boundary layer displacement thickness

δ2m boundary layer momentum thickness

δij m Kronecker delta function

σij Nm−2surface stress tensor

τij Nm−2viscous stress tensor

τs eddy characteristic timescale

εm2s−3turbulent energy dissipation

εij m2s−3turbulent energy dissipation tensor

σk- Prandtl number

φi- arbitrary variable

τWNm−2wall 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

k−ω

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

]

k−ε

model, the Wilcox [

24

]

k−ω

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

k−ε

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

0.5ρ∞U2

∞

and CL=FL

0.5ρ∞U2

∞

(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

A−B−C−D

, 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

k−ε

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

k−ε

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 + γ−1

2M2

1/(γ−1)

(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

k−ε

,

k−ω

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

∆x≥1.5(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(x−r, 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

(Ui−Ui) = 0 (2.11)

The conservative form of the ﬁltered momentum equation is

∂Uj

∂t +∂UiUj

∂xi

=ν∂2Uj

∂x2

i−1

ρ

∂p

∂xj

(2.12)

17

Theoretical Background 2.2 Computational Modelling of Turbulence

Deﬁning the residual-stress tensor as

τR

ij =UiUj−UiUj(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 =ν∂2Uj

∂x2

i−∂τ r

ij

∂xi−1

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

=εf−℘r(2.16)

where εand ℘are deﬁned by

εr≡2νSijSij (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

3kδij =−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)/ρ =−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 k−εmodel

The

k−ε

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

k−ε

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

k−ε

model, with Launder and Sharma [

35

] providing

improved values of the model constants. Focusing on the square cylinder case, the

k−ε

model was used by Bosch and Rodi [

36

] comparing it with a modiﬁcation

suggested by Kato and Launder [

37

]. There, the standard

k−ε

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

k−ε

model proposed by Kato and Launder

[

37

] avoids this problem. Nevertheless, the

k−ε

model showing a good prediction

behavior on the regions far away from the walls.

In addition to the turbulent viscosity hypothesis, the

k−ε

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/ε (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

σk∇k

+℘−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

Dε

Dt =∇ ·

νT

σε∇ε

+Cε1

℘ε

k−Cε2

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

σk∇k

+℘−ε(2.26)

∂ε

∂t +hUi · ∂ε

∂xi

=∇ ·

νT

σε∇ε

+Cε1

℘ε

k−Cε2

ε2

k(2.27)

where ℘is the rate of production of the turbulent kinetic energy:

℘=−huiuji∂hUji

∂xi

(2.28)

Additionally, as stated by Younis and Abrishamchi [

38

] after their ﬁrst numerical

research on the square cylinder case, the

k−ε

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 k−ωmodel

According to Pope [

7

], the

k−ω

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

k−ε

model. As described in detail by Wilcox [

24

], the

k−ω

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

Dω

Dt =∇ ·

νT

σω∇ω

+Cω1

℘ω

k−Cω2ω2+2νT

σωk∇ω· ∇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

k−ε

and

k−ω

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

k−ω

model in the near wall region, and to take advantage of the freestream

independence of the

k−ε

model in the outer part of the boundary layer. To achieve

this, the

k−ε

model is transformed into a

k−ω

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 k−εmodel:

Dk

Dt =∇ ·

νT

σ0

k∇k

+℘−ω(2.30)

Dω

Dt =∇ ·

νT

σ0

ω∇ω

+C0

ω1

℘ω

k−C0

ω2ω2+2νT

σ0

ωk∇ω· ∇k(2.31)

Original k−ωmodel:

Dk

Dt =∇ ·

νT

σ00

k∇k

+℘−ω(2.32)

Dω

Dt =∇ ·

νT

σ00

ω∇ω

+C00

ω1

℘ω

k−C00

ω2ω2(2.33)

Then, the modiﬁed energy dissipation Eq. (2.31) and the turbulence energy Eq.

(2.30) from the

k−ε

model are multiplied by

F1

and Eq. (2.32) and (2.33) from the

k−ω

model are multiplied by (1

−F1

). Finally, the corresponding equations of each

set are added together to give the new model:

Dk

Dt =∇ ·

νT

σk∇k

+℘−ω(2.34)

Dω

Dt =∇ ·

νT

σω∇ω

+Cω1

℘ω

k−Cω2ω2+ (1 −F1)2νT

σωk∇ω· ∇k(2.35)

Let

φ1

represent any constant in the original

k−ω

model (

σ00

k, σ00

ω

,

C00

ωi

, ...),

φ2

any

constant in the transformed

k−ε

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 ≡=−huiuki∂hUji

∂xk− hujuki∂hUii

∂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 ≡ν∂huiuji

∂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

k−ε

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 k−εby 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

k−ε

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:

dφ

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/η

= 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∞=ρ∞U∞Hcyl

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 ·10−5273,15 110,4

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=u∆t

∆x≤Cmax (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=Cmax∆x

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