MSc Thesis - Luis Felipe Paulinyi - Separation Prediction Using State of the Art Turbulence Models
1. University of Southampton
Faculty of Engineering and the Environment
MSc. Race Car Aerodynamics
Separation Prediction Using State of the
Art Turbulence Models
Luis Felipe de Aguilar Paulinyi
Supervisor: Richard D Sandberg
Second Assessor: John S Shrimpton
Southampton
September 2013
5. Acknowledgments
This thesis is the last building block of an amazing journey that I had throughout
this year and I would like to acknowledge and thank from the bottom of my heart the
contribution of the following individuals:
My wife, son and daughter, for understanding and for being there for me;
My mother, for the psychological and financial support;
My brother, a great motivator;
Professor Richard Sandberg, for sharing his knowledge and for his guidance during this
project;
My colleagues and friends: Richard Prichler, Jack Whetheritt, Jesus Pozo, Manuel Diaz
Brito, David Williams and Paulo Gustavo Cervantes for all the help in this project.
v
6.
7. Abstract
A computational fluid dynamics (CFD) examination of the flow over the two-dimensional
T106 turbine cascade blade was conducted using the Reynolds Averaged Navier-Stokes
(RANS) equations with different turbulence models using OpenFOAM as the solver. By
being an open source solver, OpenFOAM gives an unparalleled flexibility in defining the
problem setup when compared with other commercial software, this flexibility allows the
programming of new modules such as different turbulent models from the ones provided,
which allowed the investigation of two state of the art Explicit Algebraic Stress Models
(EASM), a baseline EASM and the ϕ-α-EASM and compare them with classic turbulence
models such as Spallart-Almaras and k-ω-SST. Classical turbulence models based in the
Boussinesq hypothesis, by not being able to describe stress anisotropy, usually fail to
produce accurate results in flows with high streamline curvature such as the T106 blade.
Two different Reynolds number conditions were tested 60,000 and 150,000. At the lower
Reynolds number the use of the ϕ-α-EASM model have shown a better agreement with
experimental and direct numerical simulation (DNS) results for most of the regions of
attached flow and favorable pressure gradient, however, it failed to predict flow separation
due to the reduced Reynolds number, where laminar flow simulations presented better
results.
15. Nomenclature
αp The under-relaxation factor applied to the pressure
∆t The time step in an unsteady simulation
δ Boundary layer thickness
δij Kroeneker delta
Γ An Interface diffusion coefficient
N The Navier-Stokes operator
µ Molecular viscosity
µt Turbulent eddy viscosity
νt Kinematic turbulent eddy viscosity
νTo Clauser turbulent viscosity in the outer layer
Ω(y) The wake loss at a determined the non-dimensional height y at 40% chord down-
stream
Ωij The transport of Reynolds stresses due to rotation
φ A general vector or scalar variable
Πij The transport of Reynolds stresses due to turbulent pressure-strain iterations
τ Shear stress
V Volume
εij The rate of dissipation of Reynolds stresses
C The Courant number
Cp The pressure coefficient
Cijk Turbulent transport tensor
Cij The transport of Reynolds Stresses by convection
D Diameter
Dij The transport of Reynolds Stresses by diffusion
FE Ensemble average function
xv
16. xvi LIST OF TABLES
FT Time average function
FV Volume average function
k Turbulence kinetic energy
lmix Mixing length
N number of separate experiments
P Mean static pressure
p Instantaneous static pressure
p Correction for pressure field in the solution of pressure-velocity coupling algorithms
p∗
Guessed pressure field in the solution of pressure-velocity coupling algorithms
Pij The rate of production of Reynolds Stresses
Ps The static pressure
Ps(x) The static pressure at a determined coordinate x on the blade
Pt The total pressure, the sum of static pressure and dynamic pressure
Rij The kinematic Reynolds stresses
Re The Reynolds number
Sφ The source term for the variable φ
sij Instantaneous strain-rate tensor
Sji Mean strain-rate tensor
T Characteristic time scale
t Time
tji Instantaneous viscous stress tensor
ui, uj Fluctuating velocity in tensor notation
U, V Mean velocity component in x and y directions
Ui, Uj Mean velocity in tensor notation
ui, uj Instantaneous velocity in tensor notation
vmix Mixing velocity
xi, xj Position vector in tensor notation
A Area
CV Control Volume
l A characteristic turbulence length
q A characteristic turbulence velocity
SC Control surface
17. Chapter 1
Introduction
1.1 Overview
The science of fluid mechanics has accompanied mankind since antiquity; the knowl-
edge of fluid behavior and successful management of fluid forces led to the survival of
early civilizations. Even if the concept of the aqueduct were developed independently in
different parts of the planet and by different civilizations, the Roman aqueduct is prob-
ably one of the best examples of the use of systematic engineering knowledge in fluid
mechanics applied to the construction of large-scale civil works to sustain the expansion
of the population in the roman cities.
Knowledge of fluid behavior and the correct estimation of the forces involved in certain
phenomena also led to competitive advantages as pointed out majestically by Anderson[1]:
the early aircraft developed in the beginning of the XX century employed very thin airfoils
in their wings, which resulted in poor high-lift performance due to separation at low angles
of attack, however, the research developed by Ludwig Prandtl on 1917 have shown that
the use of a thicker airfoil would be advantageous and the concept was implemented by
Antony Fokker in the Fokker Dr-1 and later on the Fokker D-VII which outperformed its
opponents during the First World War.
In competitive industries such as the aircraft, energy generation or race car industries,
the speed of reaching a solution that will meet the needs of the consumer or give a better
performance in an ever changing regulations environment could be vital to the survival
of a company or a team. The need of efficient ways to reach an improved solution is even
more important in the current scenario of an economic recession.
One good example of the need to obtain a solution with improved performance in the
fastest time and the smallest effort possible in the race car industry is Formula 1, where the
International Automobile Federation (FIA) has imposed restrictive rules regarding wind
tunnel, track tests [2] and CFD simulations, to avoid the escalating expenses of the teams.
In the specific case of CFD studies there is a limit on the number of Teraflops allowed
for each team [3]. In other industries it is not much different from racing cars; instead
of crossing the finish line first it is necessary to have the fastest time to market. In the
aircraft industry, the enforcement of noise regulation in various parts of the world created
the demand of an aircraft with reduced noise, which created a tremendous technical and
scientific effort in the area.
One of the most important problems in practical aerodynamics is the determination of
the position of the boundary layer separation. The presence of adverse pressure gradients
will result in a reduction of the velocities on the boundary layer up to a point where the
velocity gradient on the surface is zero. The knowledge of this position is important since
1
18. 2 CHAPTER 1. INTRODUCTION
the flow after the separation is dominantly rotational, causing changes on the pressure
distribution over the body and an increase on the drag, therefore, the point of the flow
separation is a very important consideration in any aerodynamic design.
This problem becomes particularly relevant in the design of Low Pressure Turbines
(LPT), where the overall efficiency of a gas turbine is highly dependent of the efficiency
on the LPT stage. An increase in 1% of the polytropic efficiency of the LPT can lead to a
reduction in up to 0.5% in the fuel consumption of the turbine, therefore a lot of research
has been directed in obtaining a more efficient design for the aerodynamic profile of that
stage and an increase of 13% in its efficiency has been obtained in the past 50 years [4]. In
such a long timespan the methodology used in designing these components has changed
considerably especially when considering the role played by the numerical simulations.
Having dependable techniques to estimate the fluid forces is a fundamental need in the
aeronautical industry, and the evolution of the computing power associated with the new
numerical methods developed caused a shift of paradigm on aerodynamic calculations.
The first step was the implementation of the potential methods for solving airfoils. To
estimate flow properties using these methods could be a quite difficult task since most
of the software had to be developed by the research group itself, as stated by Liebeck in
his 1978 paper [5] that the lack of a multi-element inverse method to solve the pressure
distribution over an airfoil had impaired the obtention of better results. Also the need
of a considerably good computer even in geometries with a few hundred of panels can
be realized in the reference document of the XFoil Software [6], developed in 1986 which
recommends the use of the software in a good workstation, otherwise the solution could
take too long.
In 1989, Cebeci et al. [7] said that the limitations on the computer power demanded
that most of the development of an aircraft was made by wind tunnel testing with flow
calculation methods being responsible for a small contribution on simple geometries. The
available numerical approaches at that time were the use of coupling techniques between
inviscid and viscous flows solving the boundary layer equations close to the solid surfaces
and the solution of the Reynolds Averaged Navier Stokes Equations (RANS) in meshes
with 5×105
cells, which can be very stringent to the type and size of geometry that is
going to be simulated. The author also states that the results obtained with the first
method were reasonably accurate at low angles of attack and only took a fraction of the
thin-layer Navier-Stokes equations calculations.
Nowadays the use of some form of simulation using RANS models is almost an indus-
trial standard. The evolution from sparse in-house codes to commercial packages with a
user-friendly interface combining mesh-generation and post-processing allowed a massive
increase in the number of users of this tool. In the past ten years the use of CFD by
Formula 1 teams jumped from a couple of full models run a year to hundreds of jobs in a
week [3], and the evolution in the solutions obtained is not restricted to a faster turnover,
the way in which turbulence is modelled is also constantly evolving.
According to the purpose of simulation that is being performed the use of an average
solution will not capture the desired details of the flow field under study, whether be-
cause the phenomenon under study is intrinsically unsteady or because knowledge of the
instantaneous flow features is needed. The ratio of how much turbulent kinetic energy is
modelled compared with how much is calculated by the solver is normally used to classify
the type of turbulence modelings. By modeling most of the turbulent spectrum RANS
models can provide an averaged flow field, and be less computationally demanding. Large
Eddy Simulation (LES) models compute most of the energy-containing scales of turbu-
lence and model most of the dissipative scales, with increased computational cost. Direct
19. 1.1. OVERVIEW 3
Numerical Simulation (DNS) simulates all of the turbulence spectrum, being the most
demanding method in terms of computing power.
To simulate all turbulence spectrum, DNS simulations must have a mesh refined enough
to capture the turbulence micro scales. As an example on how demanding a DNS cal-
culation can be when compared to RANS, the simulation of the flow over an automobile
can be used: in the RANS simulation of a 1/3 size model race car at 30 m/s Giovanetti
et al. [8] have used a 12.5 million cells mesh, the most refined cells were in the boundary
layers with approximately 1 mm thick using wall functions. Wilcox [9] estimates the size
of the turbulent micro scales near the driver’s windows in an automobile at 29 m/s as
approximately 4.6×10−3
. Since in DNS the mesh must be sufficiently refined to calculate
the micro scales a simplified analysis would estimate a mesh 2193
≈ 1.5 × 106
times more
refined. These results are discouraging when considering DNS simulations as an indus-
trial standard. By comparing the ratio between the large and small scales it is possible
to calculate the computational cost for a DNS method as proportional to Re9/4
, which
restricts its applications to specific problems at reduced Reynolds numbers.
Another comparison is given by Fr¨ohlich and von Terzi [10] that states that an LES
simulation is 10 to 100 times more costly than RANS computations, however Gadebusch
[11], is optimistic by stating that the technological advances in supercomputing are allow-
ing the LES simulations to become a useful engineering tool to predict turbulent flows.
While becoming more accessible, LES simulations also suffer from the computational ef-
fort scaling with the Reynolds number with a smaller constant than DNS [12], especially
when solving wall-bounded flows, since close to the wall the structures that carry most
of the energy become very small. Therefore it seems straightforward to think that some
computation power could be saved by solving a RANS model in the near wall region and a
LES model to solve the outer region of the flow. This and several other ways of using dif-
ferent turbulence modeling to different parts of the flow are grouped as DNS/LES/RANS
hybrid models.
The accessibility of the LES simulation or the hybrid models is in fact getting closer
to industrial application, commercial packages such as STAR-CCM+ already offer the
possibility of modeling the turbulence using either LES or a Detached Eddy Simulation
(DES) which is a hybrid LES/RANS simulation that uses the RANS modeling for the
shear layers and a subgrid scale model where the mesh is enough refined [13] .
The use of a commercial package however presents some limitations: the user is
bounded by the implemented solvers and turbulence models. The viable alternative is
the use of Open Field Operation Manipulation CFD Toolbox (OpenFOAM), which is an
open source CFD package developed by ESI-OpenCFD, a company based in Bracknell,
UK, established in 2004. OpenFOAM has several modules implemented that allow the
user to solve problems ranging from electromagnetics and solid dynamics to turbulent
flows. By being an open source software it allows the possibility of customizing its mod-
ules. The software also allows the user to select the level of turbulence modeling; it can
perform RANS, LES, DNS and also the hybrid DES.
As shown previously, advances in computational power are gradually allowing the pos-
sibility of performing an even more complex range of flow simulations in industrial applica-
tions, yet the most refined modeling, such as LES and DNS, still present some limitations
of practical order, therefore, a tool for accurately predicting the flow separation with a
reduced computational cost is highly desirable. Designers can take advantage of the fast
response of one of the novel RANS models that can accurately predict the turbulent flow
behavior and save precious CPU time to analyze new and untested geometries.
20. 4 CHAPTER 1. INTRODUCTION
1.2 Motivation
The use of the RANS models to predict a complex phenomenon such as the flow
separation in aerodynamic surfaces demands a good experimental database or reliable
DNS results as benchmark data. The University of Southampton has a long tradition of
research in race car aerodynamics. The University’s R. J. Mitchel wind tunnel was used by
different Formula 1 and IndyCar teams in the past and many of the University’s former
students are currently working in Formula 1 teams. Within this partnership between
the University and Formula 1 teams, the original subject of the present thesis was the
prediction of separation of the boundary layer on a race car related geometry, however,
due to the difficulty of obtaining a suitable geometry with experimental data to develop
the studies, a change of path was made and the study of a LPT profile was undertaken.
The study of LPT is also a very active topic of research at the University of Southamp-
ton, with several recent studies being developed, especially using DNS to solve the flow,
which gives a richness of data, such as meshes and numerical results, that can be used to
develop the current study and to compare the results.
Gas turbines are used in a wide range of applications, in the propulsion of different
types of aerial vehicles from big airliners to cruise missiles and in the generation of en-
ergy. They are attractive in some applications due to their higher power-to-weight ratio,
higher efficiency and smaller size when compared to reciprocating engines of the same
power. These benefits come with an additional cost, gas turbines also operate in a higher
temperature and velocity environment which demands a far more complex design and
manufacture.
Turbines are the last stage in a gas turbine; their main function is to transform the
energy from the high pressure gas that comes from the combustion chamber in shaft work
output. In order to extract most of the energy from the flow, turbines are designed with
multi-stages, and through the stages the flow pressure reduces hence the later stages of a
gas turbine are nominated the low pressure turbine. The overall efficiency of the turbine
is strongly dependent on the LPT efficiency, in order to reduce the fuel consumption in
jet gas turbines two possible methods can be used: the first is increasing the efficiency of
the turbine blades; the second way is to reduce the number of blades, with the associated
reduction in the mass of the engine and consequent reduction in consumption. This last
approach leads to higher loading and pressure gradients at which the individual blades
will be subjected, which demands the use of more resistant materials.
Since the present thesis is the concluding work of a MSc. in Race Car Aerodynamics,
a comparison between similar characteristics of the flow in a LPT and a race car seems
to be appropriate. In aircraft LPT, according to Stieger [4], the Reynolds numbers based
on the blade chord can range from approximately 4 × 104
to 5 × 105
depending on the
size of the engine and the altitude; when analyzing the flow on the rear wing of a race
car the Reynolds numbers can range from zero to 1 ×106
depending on the size of the
wing chord and velocity of the car. By being the last stage in a gas turbine, the flow that
reaches the turbine blades is highly disturbed due to interactions with previous stages;
similarly the flow that reaches some components of a race car such as the rear wing are
highly disturbed and rotational by the influence of other aerodynamic structures of the
car or by the effect of a car in the front. The aerodynamic profiles in LPT are normally
highly cambered in order to extract the most of the energy from the flow, the same is true
at the rear wing of race cars, by being the last component of the car, a highly cambered
wing is used in order to obtain a great amount of downforce before the flow leaves the
car, sometimes even Gurney flaps are attached to the trailing edge to extract an extra
21. 1.3. OBJECTIVE 5
bit of aerodynamic downforce from the flow. In order to use such high cambered profiles,
gas turbines take advantage of the interaction between the successive profiles in a cascade
of blades existent in the blade ring of the LPT, a similar effect is obtained by the use
of multi element wings in race cars that allow the flow to pass through a much higher
cambered wing.
As in the race car industry, the turbo-machinery industry can also profit from accurate
RANS models predictions at the conceptual design level, according to Weinmann, M. [14],
despite the constant evolution in computing power, the use of the RANS approach will
continue to have a central role on flow simulations for industrial engineering applications in
the near future. Wissink [15] points out that DNS simulations of the low Reynolds Number
flow at the LPT, despite being feasible are still too costly for engineering applications,
therefore, DNS is being used to get a better insight on the physics of the flow and to
provide reference data for the development of turbulence models.
The attempts to develop mathematical models to describe the turbulent stresses started
with the work of Reynolds more than one century ago by the process of time averaging
the Navier-Stokes equations. From that starting point, two main approaches have been
developed, depending whether or not they use the Boussinesq hypothesis, it assumes that
the Reynolds Stresses are analogous to the shear stresses and therefore calculated based
on the velocity gradients, which simplifies the calculations and the physical phenomena.
On the other hand, by obviating the Boussinesq hypothesis, the computations suffer from
increased cost by modeling the transport of each of the Reynolds stresses.
The Bousinessq hypothesis has been used successfully in several engineering applica-
tions, however, due to its linear relationship between the Reynolds Stresses and the mean
strain-rate tensor, it is inaccurate in describing the actual response of turbulence to com-
plex mean-flow perturbations and to anisotropy in the Reynolds stresses such as: flows
over curved surfaces, flows in ducts, flows in rotating fluids, secondary flows, tridimen-
sional flow, separations and obstacles. In a real flow, the Reynolds stresses adjust to these
changes in an unrelated form to mean flow processes.
1.3 Objective
The current research will focus on one of these flows that are allegedly poorly pre-
dicted by linear turbulence models: the flow in a highly cambered T106 LPT cascade
profile and compare their performance with two modern non-linear turbulence models:
a baseline Explicit Algebraic Stress Model (EASM) and the ϕ-α-EASM. Incompressible
RANS simulations will be performed in OpenFOAM, since these modern RANS mod-
els are not available in commercial packages and were programmed into OpenFOAM in
previous research projects developed at the University of Southampton [14]. Simulations
will be compared with experimental and numerical results from compressible and incom-
pressible DNS. The performance will also be assessed by testing the models in coarser
meshes.
To reach the proposed objectives several steps had to be completed:
• learning to work in the OpenFOAM framework: the author had no previous experi-
ence with the software therefore some time had to be spent in the learning process;
• obtain a suitable mesh to execute the simulations: the development of meshes for
non conventional geometries is rather difficult in OpenFOAM, hence the mesh used
in a DNS study at the University of Southampton was employed [16];
22. 6 CHAPTER 1. INTRODUCTION
• develop a program to coarsen the mesh: to test the quality of the numerical predic-
tions in coarser meshes;
• run a series of preliminary simulations: to get confident with the results generated
by OpenFOAM;
• get the state-of-the-art turbulence models working with the available mesh: the
models were developed for an early version and recently upgraded, therefore their
functionality should be tested;
• run the proper simulations: to accomplish the ultimate objective of the thesis;
1.4 Organization of the Thesis
The present work is organized in 5 chapters. Turbulence modeling is a vast subject
hence in Chapter 1 the idea was to present a brief introduction on the subject and the
main objectives of the work in order to situate the project in the current practices on the
field. Chapter 2 presents a brief revision of the concepts and theories that were used to
develop the project. The idea was to write a concise chapter that could touch on major
issues, therefore, only the most important equations in their derived form are presented.
Chapter 3 presents the specific geometry that was studied and the mesh used to calculate
the numeric solutions, the chapter also discusses the finite volumes approach and how the
problem was set in OpenFOAM environment. Chapter 4 presents the results obtained, in
the first part of the chapter it is shown the preliminary results generated in order to learn
how to use the CFD solver and in the second part the results targeted on the objectives
are presented. Chapter 5 is the conclusion of the work and suggestions to further work
are presented.
23. Chapter 2
Theoretical Background
Since the objective of the present work is to determine the point of separation on
aerodynamic profiles, a few considerations about viscous flows were made by defining it
and explaining the mechanism of separation, also a short incursion into the vast field
of the fundamentals of turbulent flows is presented along with the basics of turbulence
modelling. For a more comprehensive discussion on these subjects, the reader is suggested
to consult the following references: Anderson [1], Wilcox [9], Houghton and Carpenter
[17], Schlichting [18], Pope [19], Davidson [20], and Mathieu and Scoot [21].
2.1 Viscous Flow
Viscosity is an inherent property of any real fluid. When a fluid is submitted to a
shear stress it will sustain continuous deformation and viscosity is the property that
relates the deformation of the fluid with the amount of shear stress exerted. It is observed
by experiment that the intermolecular interaction between solid surfaces and the fluid
ensure that the velocity of the flow at the body surface is zero, this is called the non-slip
condition, hence if a stream of fluid is passing by a solid surface, it is reasonable to admit
that the velocity close to the wall will vary from zero to the stream velocity. This is the
effect of the viscosity: at the solid boundary the flow velocity is zero, this layer of fluid
will act on the following layer of fluid by generating a frictional force that will reduce its
velocity and each adjacent layer of fluid will have a decelerating effect on the following
layer up to a point where the effect of viscosity is so small that the flow velocity reaches the
stream velocity. By the action of Newton’s Third Law, the effect of viscosity on the fluid
is its deceleration by the formation of a distribution of velocities from zero to the velocity
of the stream, and the effect on the solid boundary is the appearance of a tangential
force in the direction of the flow. For newtonian fluids, the viscosity is the constant of
proportionality between the shear stress and the gradient of velocity as follows:
τ = µ
du
dy
(2.1)
The variation of fluid velocity from zero to the free stream velocity in a region close to
a solid surface is called boundary layer and its discovery was one of the most significant
breakthroughs in the science of the fluid mechanics. For a long time, the connection
between the empirical science of hydraulics and the theoretical fluid mechanics was lacking
a theory that could unify both fields of knowledge. Several practical problems could be
solved without considering the viscous effects on the fluid, since the velocity gradients
7
24. 8 CHAPTER 2. THEORETICAL BACKGROUND
are negligibly small throughout most of the fluid, however, some problems could not be
solved properly because the velocity gradients are considerable in the area immediately
adjacent to the solid boundary and consequently generates high shear stress. Prandtl
developed the concept in 1904, stating that a variation on the flow velocity from zero to
the free stream velocity is expected in a very thin region close to any solid boundary and
that difference on velocity could lead to a high shearing stress. The drag force1
felt in
bodies immersed in a flow is mainly from the shearing stresses on the surface of the body,
therefore the knowledge of the behavior of the boundary layer and consequent estimation
of these stresses is fundamental to the accurate prediction of drag. Boundary layers can
start on a sharp edge, e.g., the leading edge of a flat plate or at the stagnation point of
the leading edge of a bluff body and it will grow from zero to a finite thickness, as the
fluid flows downstream and the shear stress causes a deceleration of the layers of fluid
adjacent to the wall, the size of the area affected by the shear stress will increase, therefore
boundary layers growth in the stream wise direction.
When passing close to a solid boundary, the flow can be subjected to pressure gradients
that will affect the flow within the boundary layer. Considering the situation where the
pressure decreases in the direction of the flow, it can be expected that the pressure forces
will act against the viscous forces. An element inside the boundary layer would have a
higher velocity when compared with a case with no pressure gradient, this is said to be
a favorable pressure gradient. The flow is not decelerated as intensely close to the solid
surface, a fuller velocity profile is developed and the boundary layer grows more slowly.
In the case of the pressure increasing in the direction of the flow, the pressure force will
add to the effect of the viscous forces and a lower velocity when compared with the case
of zero pressure gradient is expected, this is said to be an adverse pressure gradient and
the boundary layer will grow faster. The deceleration of the fluid particles can become so
intense that the velocity can reach zero or even become negative. This effect is illustrated
at Figure 2.1a, it can be seen that while moving downstream the velocity profile close
to the surface becomes less inclined up to a point where the inclination is zero, further
increase of the pressure causes a reversed flow. The consequence of this reversed flow is
the separation of the boundary layer from the solid surface and the formation of a wake
of recirculating flow downstream that can be seen in Figure 2.1b. The point where the
inclination of the velocity profile is zero is defined as the point of separation. In that
point the shear stress is zero. The separation of the boundary layer causes an alteration
on the flow field and the pressure distribution over the body, in the aerodynamic jargon it
is said that the flow does not “see” the body shape as it is but “sees” an altered effective
body, thicker than the original body due to separation. As it could be expected a change
in the pressure distribution will cause an increase of the aerodynamic drag and it is called
pressure drag.
Changes on the pressure distribution over the body due to separation can lead to
undesirable results on aerodynamic profiles. A sudden increase of pressure on an airfoil can
compromise most of the lift generated reducing its efficiency or even rendering it useless,
hence, the careful management of the airfoil geometry in order to obtain a suitable pressure
distribution is the key to design efficient aerodynamic devices, as mentioned in Section
1.2, the efficiency of the LPT stage is fundamental to the design of more economical gas
turbines, so the efficient design of the LPT profile is a crucial task in gas turbine design.
As the flow interacts with a solid wall, two different flow regimes are possible on
boundary layers, the laminar and turbulent. In the laminar regime, the flow is the smooth
movement between laminae (layers) that are decelerated by the viscous action of the fluid
1
The drag force caused by the viscous stresses is also called skin friction.
25. 2.1. VISCOUS FLOW 9
(a) Vector Field
(b) Line integral convolution
Figure 2.1: Flow close to a solid surface under the influence of an adverse pressure gradient,
the deceleration of the flow leads to a reversed flow and a consequent separation
between the layers resulting in a well behaved velocity profile, in the turbulent boundary
layers there are fluctuations of velocity in the direction of the flow and perpendicular to
it, the perpendicular fluctuations transport mass between adjacent layers and makes the
velocity profile change in time. Since the velocity profile varies in time, a time averaged
velocity profile can be obtained, the movement between the layers of fluid bringing high
momentum flow from higher layers of the boundary layer to lower layers makes the average
velocity profile fuller than the laminar profile. Figure 2.2 shows the laminar profile and
the turbulent averaged profile obtained from numerical simulations, in the figure, the scale
of the vectors is different in each case, nevertheless it is possible to see the difference on
the shape of the profiles.
In general, when the flow starts its interaction with a solid boundary it is laminar, as
it proceeds further downstream, internal instabilities starts to be formed and amplified,
this process continues up to a point in which the flow can no longer sustain its smooth
and laminar movement, and it suffers a transition to a turbulent flow. According to
Equation 2.1, the fuller turbulent profile indicates that the shear stress on the wall will
be higher than the laminar case, therefore, an increase on the drag of a body immersed
on the flow can be expected. Nevertheless, turbulent profiles are more energetic and less
prone to separation than laminar profiles, consequently the determination of the regime
in which an aerodynamic profile will work is another important design decision, since a
trade-off can be obtained by working in the turbulent regime with a higher skin friction
and without any flow separation instead of in a laminar regime with lower skin friction
with a greater tendency to separation.
26. 10 CHAPTER 2. THEORETICAL BACKGROUND
(a) Laminar boundary layer (b) Turbulent boundary Layer
Figure 2.2: Results obtained numerically for the velocity distribution on the boundary
layers.
2.1.1 The Navier Stokes Equations
The equations that describe the behavior of nearly all fluids are called the Navier-
Stokes equations due to the work of the French engineer Claude-Louis Navier and the
Irish mathematician George Gabriel Stokes. They are a set of nonlinear partial differen-
tial equations that represent three fundamental physical principles: conservation of mass,
Newton’s second law and the conservation of energy. According to Davidson [20], the
Navier Stokes equations are “deceptively simple”, as they don’t look more complex than
a wave equation or a diffusion equation, which in the author words, “leads to simple solu-
tions”. For him, The Navier-Stokes equation “embodies such rich and complex phenomena
as instabilities and turbulence” as a consequence of a “seemingly innocent non-linearity”
of the dependent variable in quadratic form.
For the incompressible flow of a Newtonian and continuum fluid, the equations of the
conservation of mass and momentum are:
∂ui
∂xi
= 0 (2.2)
ρ
∂ui
∂t
+ ρuj
∂ui
∂xj
= −
∂p
∂xi
+
∂tji
∂xj
(2.3)
the equations are presented using the subscript notation, with the subscripts taking
the values of the x, y and z components and with the summation convention employed,
where a single term containing one or more repeated subscripts represents an implied sum
over all three values of each repeated subscript. The viscous stress tensor, tij, and the
instantaneous stress tensor sij are defined as:
tij = 2µsij (2.4)
sij =
1
2
∂ui
∂xj
+
∂ui
∂xj
(2.5)
27. 2.2. TURBULENCE FUNDAMENTALS 11
2.2 Turbulence Fundamentals
A precise definition for turbulence is often tried by different authors, but often a concise
definition cannot encompass all its complexity. Some of the greatest minds from Leonardo
da Vinci to Richard Feynmann have been puzzled by its characteristics and some even
used poetry to try to express their comprehension over the subject, like the famous verse
of the British mathematician Lewis Richardson2
.Despite being a phenomenon that is part
of people daily lives, it has been a challenge and authors rather try to introduce turbulence
by its general properties.
As it was mentioned in section 2.1, turbulence arises from instabilities of laminar flow.
The earliest contributions on the subject are owed to the pioneering work of Osborne
Reynolds over the behavior of the flow in pipes and how it could change based on pertur-
bations on the inlet and a parameter, later named as the Reynolds number, as follows:
Re =
ρ UD
µ
(2.6)
The Reynolds number gives a measure of the ratio between the inertial forces and the
viscous forces in the flow, an increase in its value, corresponds to an increase in the relative
importance of the non-linear convective term on the right-hand side over the viscous term
on the left-hand side of Equation 2.3. The viscous term tends to damp the instabilities
within the flow and with not enough damping an increase of the flow internal instabilities
will occur.
Considering the flow on a pipe, in the laminar regime the velocity profile is parallel to
the axis of the pipe and has a parabolic distribution, which is a possible solution for the
Navier-Stokes equation. It was observed that the viscosity tends to damp the perturba-
tions on the flow up to a certain Reynolds number, when it is increased, the tendency to
instability increases and the flow starts to suffer a transition by having sporadic bursts
of turbulence. As the Reynolds number is further increased a fully turbulent regime is
attained, with the parallel velocity profile being substituted by rotational flow structures.
It is important to notice that the instabilities by themselves are not an indication of a
turbulent regime, one of the best examples of instabilities developing in a laminar flow is
the formation of the Karman vortex street on a cylinder, the vortex wake is formed by an
unsteady separation of the boundary layers on the top and bottom sides of the cylinder,
as the flow Reynolds number is increased the transition to turbulent flow begins to form
on the far wake of the vortex street. Despite the fact that there are some conditions for
a turbulent flow to develop and that viscosity also contributes to damp instabilities on
the flow that can even lead to a relaminarization, the laminar flow is more an exception
than a rule, as it said by Wilcox [9]: “Virtually all flow of practical engineering interest
are turbulent”, mentioning several applications in which turbulent flow is present from
the flow past vehicles to the mixing of the cream in a cup of coffee. Still quoting the
author, “Turbulent flows occurs when the Reynolds number is large”, and “large” most of
the times “correspont to anything stronger than a tiny swirl, a small breeze or a puff of
wind.” The equations 2.2 and 2.3 also describes the turbulent flow. In order to obtain a
solution, these equations must be supplied by the appropriate initial and boundary condi-
tions, which for a particular set of these conditions is unique, nevertheless when executing
experiments one might never be able to reproduce the same flow due to the sensitivity to
2
“Big whorls have little whorls, which feed on their velocity,
little whorls have lesser whorls, and so on to viscosity.”
28. 12 CHAPTER 2. THEORETICAL BACKGROUND
changes in the initial and boundary conditions that cannot be controlled experimentally
with infinite precision, therefore, the theoretical study of turbulence is based on the flow
statistics, which are assumed to be reproducible by sampling a large number of differ-
ent realizations. The main turbulence properties pointed out by the above mentioned
references are:
• Turbulence is a random process: when observing the graph of the measured in-
stantaneous velocity obtained by a probe in a turbulent flow, as in Figure 2.3, one
can observe random fluctuations as a function of time. Turbulent flow is time and
space dependent and highly sensitive to initial conditions which makes its instanta-
neous properties very difficult to predict, therefore, a statistical approach is used to
describe the flow since the averaged flow properties are reproducible.
• Turbulence has a wide range of different scales: looking again at Figure 2.3, it is also
possible to see that there are large oscillations on the measured value of velocity and
within these oscillations smaller oscillations exist, this reflects the movement of large
structures passing by the probe and while they are passing smaller structures that
are living inside the large ones cause smaller fluctuation in the measured velocity.
The large scales of the flow are typically defined by the geometry, for example, in the
a jet flow they are of the order of magnitude of the width of the jet. It is possible to
determine the smaller scales in turbulence by magnifying the time interval of Figure
2.3, eventually it is possible to reach a timescale in which the oscillations in velocity
are smooth, this is due to the action of viscosity, therefore, the smallest scales on the
flow depend on the viscosity. Flow instabilities continuously generates turbulence
at high Reynolds number, producing large scale eddies which are also unstable and
form smaller ones, that also form yet smaller eddies in a continuous energy cascade
up to a point where viscosity becomes important. There is a continuum of spatial
scales generated by this energy cascade process, and the spectra get wider as the
Reynolds number increases since the dissipative smaller scales become smaller at
larger Reynolds numbers.
• Turbulence dissipates energy: as a result of the cascade process viscous flows rapidly
dissipate energy as the viscous stresses tend to have it major contribution at the
smaller scales. Turbulent flows require a continuous supply of energy, which is given
by the large scales on the flow.
• Turbulence is a continuum phenomenon: the smallest scales in a turbulent flow are
many orders of magnitude larger than the molecular free path, therefore, turbulent
flows can be described within the same continuous approximation used for deriving
the Navier-Stokes equations.
• Turbulence is intrinsically tridimensional: turbulence has a rotational nature, vortex
lines form inside of a turbulent flow and they tend to evolve by the action of the strain
rate produced by the velocity gradients in a phenomenon called “vortex stretching”.
This is one of the fundamental processes in a turbulent flow and it does not occur
in two-dimensional flows.
• Turbulence mixing and diffusivity: by the existence of large structures moving in a
turbulent flow, large masses of fluid migrate across the flow. These large structures
carry small disturbances within them, this movement greatly increases the mixing
and diffusion in a turbulent flow. Another observable phenomenon is the interaction
29. 2.3. TURBULENCE MODELING 13
Figure 2.3: Measurement of the instantaneous velocity with a probe in a turbulent flow
[26]
with neighboring regions of laminar flow, in which fluid from the surroundings is
brought into the turbulent region and as an effect a spreading of the turbulent flow
occurs in the flow direction, as is seen in a wall boundary layer.
2.3 Turbulence Modeling
According to Pope [19], the objective of the study of turbulent flows is to obtain a
quantitative theory or model that can be used to obtain results to calculate flows of
practical interest. If, in one hand, experience shows that there are no simple analytic
theories that could be applied to solve turbulent flows, on the other hand, the evolution in
computing power of digital computers allows to solve flows with increasing complexity and
detail. Nevertheless turbulent flows present several challenges that must be addressed, for
instance its tridimensionality, time dependency and randomness are characteristics that
make it difficult to develop an accurate model, moreover the large scales are intrinsically
dependent of the geometry of the flow which makes each different problem unique.
It is a fact that even before the extensive use of computers to solve turbulent flows, the
necessity to predict the behavior of such flows demanded the development of analytical
and experimental methods. One good example of analytical methods was the integral
momentum equation, derived by Von K´arm´an, that allowed practical solutions for some
engineering problems, such as the determination of momentum thickness in a turbulent
boundary layer over a body. Other analytical methods using simplified equations, experi-
mental results and actual performance data from prototypes were also applied in industry
in the past and are still in use today. A compendium that collects several methods for
aircraft design is Roskam Airplane Design Collection [22]. As an alternative, performing
experiments in different geometries at different flow regimes produced a large number
of charts, tables and practical handbooks such as the classic Hoerner’s Fluid-Dynamic
Drag and Fluid Dynamic Lift [23], [24], that were used in early stages of development of
aerospace products [25].
There is no doubt that the use of these methods allowed the execution of great engi-
neering feats; however, the simplicity of setting up a numerical simulation in graphical
interfaces, its increasingly accuracy due to the implementation of improved numerical
methods and turbulence models, and the easier access to solvers, makes the use of numer-
ical modeling every day more attractive. A short review of the main issues in numerical
modeling of turbulence will be presented in the following subsections.
30. 14 CHAPTER 2. THEORETICAL BACKGROUND
2.3.1 Turbulence Closure Strategies
Using the numerical simulation approach three different methods can be used to solve
turbulence:
• Reynolds-Averaged Navier-Stokes (RANS) models: The Navier-Stokes equa-
tions are time averaged in order to obtain a mean velocity field. In the process of
averaging the extra terms that appear are modeled. The current work was devel-
oped using RANS models therefore a more complete explanation will be performed
in subsequent sections.
• Large Eddy Simulation (LES): The idea behind LES is to solve the large scales
of turbulence while scales below a certain size are modeled. It is important to notice
that all turbulent scales are dynamically significant on turbulent flows, hence the
smaller scales must be accounted for in the model, this is made by subgrid terms that
are added to the equations of motion. This approximate approach is used in order to
reduce computational cost and allows the use of a coarser mesh. The Navier-Stokes
equations are solved to determine an instantaneous realization of the flow instead of
an average field. Since some of the smaller scales are not being calculated, LES can
only produce statistical results independent of these scales, such as mean velocity
field and second order velocity moments. According to Matieu and Scott [21], “The
art of LES lies in the appropriate choice of subgrid terms, matched to the particular
flow and numerical scheme used”, because in a real flow the turbulent energy cascade
is responsible for transferring the energy from the large scales to viscous dissipation
in a LES the size of the grid makes the energy cascade incomplete (it works up
to the scales described by the grid resolution) hence the choice of the numerical
scheme can include an artificial numerical dissipation and the subgrid turbulence
model must be selected in order to represent the correct energy transfer otherwise
the flow can become under-dissipative or over-dissipative.
• Direct Numeric Simulation: In this approach the unsteady and tridimensional
Navier-Stokes equations are also solved for an instantaneous realization of the flow
and for all turbulent scales. Since none of the scales will be modeled, the mesh
must be sufficiently refined to capture the smallest spatial scales, the time marching
must have time steps short enough to capture the period of the fastest fluctuations,
therefore, the method is costly and as it was mentioned earlier the cost increases
with the increase of Reynolds number. Due to the fact that no approximations are
being employed, except the ones related to discretization, the solution of the flow
fields yields detailed information of instantaneous and statistical properties, which
rises a concern related to storage and treatment of obtained data. In the early stages
of development of DNS techniques, the researchers were concerned in showing that
it was possible to simulate a flow accurately, nowadays the level of confidence has
increased to a level that it can be also called a “Virtual Wind Tunnel” and it allows
the execution of numerical experiments that are sometimes impossible to perform
in a laboratory such as choosing geometries or boundary conditions that cannot
be realized in practice or artificially modifying the governing equations. Alongside
with experiments, results from DNS can also provide benchmarks against which
other simulation methods can be evaluated and parametrized.
As described in the previous section, turbulent flows exist in a huge variety of appli-
cations from the flow on a cup of tea to the atmospheric flows, for such vast applications
31. 2.3. TURBULENCE MODELING 15
a large number of different models have been proposed, Pope [19] presents some criteria
that can be taken into account when evaluating different models:
• Level of description: the level of description can range from the mean flow prop-
erties to instantaneous characteristics of the flow, the use of a higher level of de-
scription leads to a deeper characterization of turbulence and a wider applicability,
its use depends on results needed for a determined application since it is more com-
putational costly, for most of the industrial flows low levels of description such as
mean-flow closures are sufficient.
• Completeness: the completeness of a model refers to its constituent equations. In
a complete model only fluid properties and boundary conditions have to be specified,
they are more costly and has wider applicability, whereas incomplete models need
the specification of other properties normally related to a specific type of flow.
• Cost and ease of use: the general trend observed when considering the evolution
of the computing power over the last decades is that the speed (number of flops) has
increased by a factor of 30 per decade, which gives and increase of approximately
106
in the last forty years. This means that in a short period of time simulations
that were regarded as research material are currently accessible to a daily CFD user.
The cost of computing a turbulent flow can be linked to several different causes: it
can vary as a result of the increase of the complexity of the flow under study or the
consideration of a more complete physical description of the phenomena; it can also
be affected by type of closure strategy selected, some models are highly sensitive
to the increase of Reynolds number, whereas in some models, the increase of cost
is insignificant of non existent; it is also important to take into account the time
employed in obtaining or developing the software to solve a particular flow and the
difficulties in operating such software.
• Range of applicability: Pope summarizes the applicability by stating “A model is
applicable to a flow if the model equations are well posed and can be solved”, there is
no point trying to obtain a shock-wave with an incompressible model nor trying to
solve a high Reynolds number flow using DNS, in the first case, the model equations
are not well posed and in the second case they cannot be solved (at least in a timely
manner).
• Accuracy: the accuracy of a certain model can be assessed by comparing its results
with experimental measurements. The discrepancies between the results can be
originated from different sources:
– Inaccuracies of the model: discrepancies can arise when the modeling equa-
tions do not correspond to the complete phenomenon under study, for example,
by using a turbulence model not suitable for a particular application.
– Numerical error: errors can arise from not using a refined enough time or
space steps or by performing calculations with insufficient numerical accuracy.
– Measurement error: results obtained from experiments have their own er-
rors.
– Discrepancies in the boundary conditions: this type of error arises from
differences between the simulated and actual boundary conditions of a prob-
lem, in some cases it is impossible to reproduce the same boundary conditions
32. 16 CHAPTER 2. THEORETICAL BACKGROUND
of a determined experiment, sometimes the boundaries are approximated or
unknown.
When performing an evaluation of the accuracy of the model it is important to
maintain the last three sources of error in a minimum level, so they do not interfere
in the conclusions of the advantages and shortcomings of the implemented model.
Sandham [27] also lists two other sources of errors: iteration errors, which is not
allowing the calculations to run far enough to reach a steady state and code errors
which are an incorrect implementation of the numerical method for the equations,
he also recommends that the results from CFD calculations should be verified to
see if the equations are being solved correctly by comparing the results with known
analytic solutions, and he adds that recently the codes can also be validated by
comparing their results against direct numerical simulations databases.
2.3.2 The Turbulence Closure Problem
As it was mentioned in the previous section, turbulence is a random process with its
average properties reproducible; hence, a statistical approach seems to be appropriate.
The averaging concept was introduced by Reynolds in 1895, and it consists in perform-
ing the averaging of the terms of the Navier-Stokes equations by decomposing the flow
quantities into the sum of a mean and a fluctuating part and substituting them into the
equations. The process of averaging the equations have the advantage of avoiding the
need of resolving all scales of turbulence, unfortunately during the process of averaging
new terms arise and they have to be modelled in order to solve the averaged equations
numerically.
In turbulent flows, different types of averages of turbulent quantities can be defined,
the most common forms are time averaging, spatial averaging and ensemble averaging.
Time averaging FT (x) of an instantaneous flow variable f(x, t) is well suited to sta-
tionary turbulence, since the majority of flows of engineering interest are stationary, this
is the most used form of Reynolds averaging. It is given by:
FT (x) = lim
T→∞
1
T
t+T
t
f(x, t) dt (2.7)
in practice T cannot be infinity, therefore, it is taken to be a period of time long enough
to capture the largest scales of turbulence that are associated with the slowest variations
of a determined flow variable. The time averaging can also be used in cases of unsteady
flows, as long as there is a separation between the period of the unsteadiness of the flow
and the time scale of the turbulence fluctuations, which is known as spectral gap. In
this case, T must be larger than the turbulence scales, but smaller than the period of the
unsteadiness.
Spatial averaging is recommended to be used in cases of homogeneous turbulence which
means that the statistics of the turbulence are independent of direction. A volume integral
is taken over a volume V in a region where turbulence is uniform in all directions:
FV (x) = lim
V→∞
1
V V
f(x, t) dV (2.8)
33. 2.3. TURBULENCE MODELING 17
Ensemble averaging, can be used for flows that can be repeated numerous times as
different individual experiments and is defined as:
FE(x, t) = lim
N→∞
1
N
N
n=1
fn(x, t) dt (2.9)
where N is the number of separate experiments using the same setup. This type of
definition is very robust since it can be applied to almost every type of turbulence problem,
however it poses a difficulty in obtaining a statistical convergence since a high number of
realizations is necessary. Other types of averages can also be defined depending on the
particular case under study.
The averaged Navier-Stokes Equations
Considering the time averaging of a stationary turbulent flow and performing the
Reynolds decomposition of the velocity it is possible to write:
ui(x, t) = Ui(x) + ui(x, t) (2.10)
Each of the variables of the Navier-Stokes equations is substituted by variables decom-
posed as shown in Equation 2.10, and the whole equation is averaged. It is important
to recall some properties of averaging such as Ui(x) = Ui(x), ui(x) = 0 and uiuj = 0.
For the full derivation of the Reynolds-Averaged Navier-Stokes Equations the reader is
recommended to refer to Versteeg and Malalasekera [28], the equations are presented in
the derived form below:
∂Ui
∂xi
= 0 (2.11)
ρ
∂Ui
∂t
+ ρUj
∂Ui
∂xj
= −
∂P
∂xi
+
∂
∂xj
(2µSji − ρujui) (2.12)
by comparing them with the Equations 2.2 and 2.3, it can be seen that the term −ρujui
arises. This term is known as the Reynolds-stress tensor, it is a symmetric tensor, hence,
in three dimensions it represents six new unknowns to the set of equations and since no
new equations have been derived, the system of equations is not closed (more unknowns
than equations) and this is known as the turbulence closure problem.
It is necessary to develop models that predict the behavior of the Reynolds stresses in
order to be able to compute flows using the RANS approach.
Employing a pure statistical analysis of the component quantities of the Reynolds stress
tensor, they can be described as the variance of the velocity fluctuations and they can
give important information on the structure of the flow. The quantities ui
2
are always
non-zero because they contain squared velocity fluctuations, and the quantities ujui are
normally non-zero and they indicate a correlation between the velocity fluctuations in
different directions, which is expected for the vortical flow structures that compose a
turbulent flow. These quantities represent momentum fluxes that are closely linked with
the additional shear stresses present in a turbulent flow.
Their effect can be understood by imagining a moving control volume within a turbulent
boundary layer. In a flow moving in the x direction forming a boundary layer, there is a
mean velocity distribution in the direction normal to the wall (y) which is responsible for
34. 18 CHAPTER 2. THEORETICAL BACKGROUND
a mean shear stress, the eddying motion through the boundaries of the control volume
continuously let in parcels of fluid with a higher or lower x-momentum, the interaction of
these parcels with different momentum with the fluid inside the control volume generates
an additional turbulent stress within the control volume known as Reynolds stresses.
2.3.3 Reynolds-Averaged Navier-Stokes Turbulence Models
The earliest attempts to model the turbulent stresses started in the 1920’s by the work
of Ludwig Prandtl when he introduced the mixing length concept which is based on the
Boussinesq hypothesis. Most of the work developed in the area in the subsequent years
was led by Prantdl, von K´arm´an and Kolmogorov and was also based on the Boussinesq
hypothesis, the most important developments where the development of models that took
in consideration the kinetic energy of turbulent fluctuations and later on a model that also
considered the dissipation of energy. It is important to mention that the development of
the models was hampered by the limitations imposed by the unavailability of computers
in that time. In the late 1940’s, Chou and Rotta started to work with a different approach
by proposing models that did not used the Boussineq approximation. This approach is
more accurate in the physical description of the phenomenon, however, it is more complex
in terms of modeling and it leads to the modeling of all the components of the Reynolds
stress tensor.
The most common didactical division to classify the turbulence models is whether they
are based or not on the Boussinesq hypothesis.
Turbulent Viscosity Models
Early experiments on turbulent theory were developed on thin shear layers like jets,
mixing layers and wakes where a causal relation between the existence of shear stresses
and the development of turbulence was postulated, it is known that the turbulence also
increases the viscous dissipation in a flow, hence an analogy was proposed by Boussinesq
that the turbulent stresses could be proportional to the mean rates of deformation just
as the viscous stresses in the Navier-Stokes equations are modeled by a viscosity times
the rate of deformation of the fluid element, as shown on Equations 2.4 and 2.5, the
Boussinesq hypothesis can be written as:
τij = −ρuiuj = µt
∂Ui
∂xj
+
∂Uj
∂xi
−
2
3
ρkδij (2.13)
µt is the eddy viscosity, it is also possible to write νt = µt/ρ, being the kinematic eddy
viscosity, and k is the turbulence kinetic energy defined as:
k =
1
2
uiui (2.14)
Equation 2.13 establishes a linear relationship between the Reynolds stresses and mean
strain rate of the flow, hence it is common to describe the turbulence models based on
the Boussinesq hypothesis as linear eddy viscosity models.
By inspecting the dimensions of the kinematic turbulent viscosity (L2
T−1
), it is possible
to say that when prescribing a specific turbulent viscosity model, it has been implicitly
prescribed a characteristic turbulent length (l) and a characteristic turbulent velocity (q)
in a way that νt = Cql, with C being a non-dimensional coefficient. Different turbulent
models have different ways of prescribing q and l and defining C as a constant or a field
variable.
35. 2.3. TURBULENCE MODELING 19
Within the turbulent viscosity models, another didactical division is made by means
of the number of equations used to calculate νt:
• Algebraic or zero-equation models: these are the simplest turbulent models
available; the turbulent velocity and length scales are calculated through algebraic
relations. These models are also classified as incomplete models since a length scale
has to be provided a priori, called the mixing length. For a series of flows these
length scales are tabulated as a function of a meaningful length of the flow. The
velocity scale must also be prescribed. The fundamentals of the algebraic models are
based on the mixing-length concept developed by Prandtl in 1925, however, some
new developments to correct some of the shortcomings of the models were made by
Van Driest in 1956, Cebeci and Smith in 1974 and Baldwin Lomax in 1978.
Despite its simplicity, these models are well established, extensively validated and
the mixing length concept proved to bear accurate results in simple two-dimensional
flows such as thin shear layers (jets, mixing layers, wakes and boundary layers) with
slow changes of direction, this is mostly because in such flows, there is a balance
in the production and dissipation and the turbulence properties are proportional to
the mixing length, which is described by algebraic formulae.
These models are cheap in terms of computing resources and easy to implement, in
an already existent laminar code, they need no more than a few extra lines to take
turbulent viscosities into account, these features make them attractive to combine
with more sophisticated turbulence models to describe wall behavior.
• One-equation models: An additional partial differential equation has to be solved.
In order to improve the prediction of the turbulent properties, Prandtl proposed in
1945 a model that related the eddy viscosity with the turbulent kinetic energy
(equation of k) and hence the concern in giving more depth to the modelling by
adding historical considerations, since the turbulent kinetic energy is affected by
where the flow has been. These models are also incomplete since a characteristic
lenght must be provided. Later on in the 1970’s and the 1990’s new one-equation
models have been proposed in which a transport Partial Differential Equation (PDE)
for νt has to be solved.
The most successful modern one-equation model is the Spalart-Almaras 1992 model,
in which a transport equation for an eddy viscosity parameter ˜ν is solved, the
length scale is specified and it determines the rate of dissipation of the transported
turbulence quantity. Due to the fact that it has only one extra PDE, it provides less
expensive calculations for boundary layers on external flows. According to reference
[28], the model constants were tuned for external aerodynamics flows and hence
they provides accurate results for boundary layers at adverse pressure gradients,
showing good prediction on stalled flows. The suitability of the model to airfoil
applications have also sparked the interest in the turbo machinery community. In
the other hand, the model proved to be unsuitable for complex geometries since it
is difficult to define an appropriate length scale, and it seems to lack sensitivity to
transport processes in rapidly changing flows.
A detailed description of the model equations is presented on the Appendix, since
this was one of the models used in the current work.
• Two-equation models: The first two-equation model was developed by Kol-
mogorov in 1942. To improve the prediction of turbulent properties he devised
36. 20 CHAPTER 2. THEORETICAL BACKGROUND
a model that apart from the equation of k also included the calculation of another
PDE for the rate of dissipation of energy. By calculating two turbulent properties,
these models does not demand the user to input specific characteristics of the flow
other than the boundary conditions. These models are also classified as complete
models. Historically, they had to wait the development of faster computers in order
to be tested and be further developed, this explains the great number of new two
equation models that have arisen after the 1970’s.
Two-equation models in general use the transport equation for the turbulent kinetic
energy k to determine the velocity scale, since q = k1/2
, different turbulent models
use different methods to obtain the length scale with the second transport equation
for the other dependent variable. These two equations allow the model to account
for flow conditions where convection and diffusion impact in the production and
dissipation of turbulence such as in recirculating flows. One of the most used and
extensively tested turbulence models is the k-ε, its second equation is the equation
of the viscous dissipation, named as ε, therefore the length scale is l = k3/2
/ε, in
this model the eddy viscosity is given by:
νt = Cql = Cµ
k2
ε
(2.15)
A detailed presentation of some of the two-equation models is also shown in the
Appendix. Close to the wall and at high Reynolds numbers, the standard k-ε model
has equations to account for the effects close to the wall (wall functions), based
on the universality of the log-law and on the fact that measurements show that the
production of turbulent kinetic energy is balanced with dissipation. At low Reynolds
numbers some modifications had to be included in the model to account for the near
wall effects.
According to reference [28], the k-ε model presented good agreement in several
industrial relevant flows, such as confined flows without the necessity of adjusting
its constants. Results with external flows, weak shear layers, axisymmetric jets in
stagnant surroundings and rotating flows are a little less encouraging. The model
also have some deficiencies that do not allow it to predict secondary flows in non
circular ducts. To address to some of the shortcomings of the standard k-ε model,
modifications have been proposed such as: the two-layer k-ε to deal with the low
Reynolds issue; the RNG k-ε model to deal with issues related to large rates of
deformation on the flow; the Wilcox k-ω and the Menter k-ω Shear Stress Transport
(SST) model to provide more accurate aerodynamic calculations, the last one was
also used in the present work.
Differently from molecular viscosity which is a property of the fluid, the turbulent
eddy viscosity is related to several aspects of the flow such as its dimensions, its geometry
and its history. The use of the Bussinesq hypothesis in the eddy viscosity models, while
giving accurate results to a range of flows, can also lead to wrong predictions even when
taking into account sophistications like the history of the flow, in fact the assumption is
a simplification and does not reflects what really happens in the flow.
These models assume that exists isotropy of the normal Reynolds stress, which is a
simplification of the real fluid behavior and it is not very accurate even in simple two-
dimensional flows such as the flow on a flat plate. In this type of modelling, the Reynolds
stress is proportional to the mean rate of strain Sij which is true in the cases where there is
37. 2.3. TURBULENCE MODELING 21
a balance on ratio of production and dissipation of turbulent kinetic energy, so it is difficult
to duplicate the actual response of turbulence to complex mean-flow perturbations with
this approach.
Non-eddy viscosity models
In view of the limitations presented in the eddy viscosity models concerning Reynolds
stress anisotropy, two main alternatives have been proposed, the Reynolds Stress Equation
Models and the Algebraic Stress Equation Models. The first originates from the work of
Launder et al. [29] in which they propose a model where each of the Reynolds Stresses is
determined from the solution of transport equations plus the solution of the equation for
turbulence energy dissipation. The second approach uses an algebraic modeling of some
of the transport terms of the Reynolds Stress transport equation reducing it to a set of
algebraic equations.
• Stress transport models: these models are also called as second-order or second-
moment closure, according to Wilcox [9] they have the “conceptual advantage”
of modeling the stress transport in a natural manner that incorporates non-local
and history effects, therefore only the initial and boundary conditions have to be
supplied without further adjustments for particular cases. The Reynolds stresses
Rij are modeled as follows:
∂Rij
∂t
+ Cij = Pij + Dij − εij + Πij + Ωij (2.16)
where:
– Rij is the kinematic Reynolds stresses
– Cij is the transport of Reynolds Stresses by convection
– Pij is the rate of production of Reynolds Stresses
– Dij is the transport of Reynolds Stresses by diffusion
– εij is the rate of dissipation of Reynolds stresses
– Πij is the transport of Reynolds stresses due to turbulent pressure-strain iter-
ations
– Ωij is the transport of Reynolds stresses due to rotation
this equation represents the transport for each one of the six individual Reynolds
stresses, they are solved along with the equation of turbulent energy dissipation
ε, hence by solving seven different partial differential equations in a tridimensional
case, this model has a higher computational cost than the models discussed previ-
ously.
The terms for convection (Cij) production (Pij) and rotation (Ωij) are used in their
exact form and the remaining terms are modelled by means of assumptions. The
diffusion term (Dij) is modeled by considering that the rate of transport of Reynolds
stresses by diffusion is proportional to gradients of Reynolds stresses; the modeling
of the dissipation rate (εij) assumes isotropy of the small dissipative eddies; the
pressure-strain term (Πij) models two different processes; a process that reduces
anisotropy that is considered to be proportional to the degree of anisotropy of the
Reynolds stresses and a process that opposes the production of anisotropic vortices
38. 22 CHAPTER 2. THEORETICAL BACKGROUND
that is taken as proportional to the production process that generate anisotropy;
the pressure-strain term contributes to the reduction of the Reynolds shear stresses
and a redistribution of energy among the normal Reynolds stresses.
According to reference [28] these models are complex, but they are “the simplest type
of model capable of describing the mean flow properties and Reynolds stresses without
a case-by-case adjustment”, they have shown to be very accurate in determining
mean flow properties and the Reynolds stresses in many flows including wall jets,
channel flows and curved flows, nevertheless they haven’t been as validated as other
turbulence models such as k-ε, they have a higher computational cost and they
are reported to perform as poorly as the k-ε in axisymetric jets and unconfined
recirculating flows due to problems with the modeling of the ε equation.
• Algebraic Stress Models (ASM): due to the high computational cost of solving
the Reynolds Stress models it was proposed that some of the terms of the Reynolds
Stress Transport Equation were modelled by algebraic expressions. This way a re-
duction of the computational effort would be achieved while still taking into account
the anisotropy of the Reynolds stresses. Gradients of the Reynolds stresses appear
in the convective Cij and diffusive Dij terms of Equation 2.16, some authors have
tested even neglecting the terms with success in some applications, but in general
the sum of these terms is replaced by the sum of the convection and diffusion terms
of the turbulent kinetic energy equation. The algebraic stress model equation is
implicit, with the Reynolds Stresses appearing in both sides of the equation, the
resulting problem was simplified from six transport equations to six algebraic equa-
tions and the solution of k and ε transport equations.
• Explicit Algebraic Stress Models (EASM): By being an implicit method, the
ASM was reported to exhibit numerical issues such as multiple solutions, singular-
ities and convergence to non-physical conditions [30]. An alternate approach is to
expand the Reynolds stresses in a series with the Boussinesq approximation as the
leading term, this will result in an explicit algebraic model, which makes them more
robust with improved predictive capabilities. Two different EASM models will be
tested within the current project, a baseline EASM and the ϕ-α-EASM, which is a
model that incorporates improved capabilities for modelling regions close to walls.
39. Chapter 3
The Problem
The problem that is being studied on the current thesis is the determination of the point
of separation of the flow through a linear LPT cascade with T106 profile sections with
RANS/URANS simulations using different turbulence models. The RANS calculations
will be performed in OpenFoam and the results will be compared with experimental and
numerical results.
Stadtm¨uller [32] performed experimental measurements of the pressure distribution and
the wake losses of the T106 blade in a low pressure linear turbine test rig with seven blades
and aspect ratio of 1.76, which was considered enough to assume a two-dimensional flow in
the middle of the blade. Due to some experimental uncertainties on the inlet conditions,
the inlet angle was estimated to be 45.5 with a Reynolds number of 59,634 and a Mach
number of 0.405. The experimental setup also had a possibility to add moving transversal
bars on the inlet that allowed him to perform experiments with incoming wakes.
Stieger [4] does an experimental study using a cascade composed by five blades with
moving bars in the inlet, to investigate the wake induced transition in separating boundary
layers. A latter study from Stieger et al. [33] investigates the fluctuation of the surface
pressure in the region of a separation bubble due to the effect of incoming wakes, and a
study from Stieger and Hodson [34] does a deep investigation on the transition mechanism
of a boundary layer in a turbine blade subjected to the effect of incoming wakes.
Due to the range of Reynolds numbers on the LPT cascades of gas turbines, DNS
studies are becoming more frequent, however, these studies are still rather expensive and
are still not accessible to a daily industrial user. The first incompressible DNS on LPT
cascades was performed by Wu and Durbin [35] where they describe the formation of two
types of longitudinal vortices caused by the passage of wakes through the LPT, they also
compare the results of DNS with LES over same configurations obtaining good agreement
for well resolved LES.
Wissink [15] performed a three-dimensional incompressible DNS over the T106 profile
with both an undisturbed inlet and a periodically disturbed inlet by incoming wakes, to
provide data for the development of turbulence models and to investigate the effect of
the incoming wakes on the boundary layer. For the undisturbed inlet case the author
executes a simulation with an inlet angle of attack of 45.5◦
and Reynolds number of
51, 831, the pitch between the blades in his study is 0.9306. The flow obtained in this
DNS simulation has a good agreement with experimental results, the author describes
the formation of a separation bubble at the leading edge of the suction side. Due to the
action of the favorable pressure gradient the disturbances originated from the unstable
leading edge separation are damped. Beyond the chord position of x/L = 0.6 the pressure
gradient becomes adverse, in the undisturbed inlet case the author reports the formation
23
40. 24 CHAPTER 3. THE PROBLEM
of constantly present separation bubble near the trailing edge (x/L ≈ 0.93), in the case
with incoming wakes the formation of an intermittent and less pronounced separation is
observed at x/L ≈ 0.87, it is a very unstable shear layer due to the effect of the incoming
disturbances.
Sandberg et al. [16] uses an in-house compressible multi-block structure curvilinear
Navier-Stokes solver to compare the flow over the T106A turbine cascade with experi-
mental data and investigate the influence of the inflow turbulence level on the transition
behavior and profile losses. They find that the laminar boundary layer separation is
strongly dependent to the level of inlet turbulence, moving downstream with increasing
turbulence level. They also observe that the turbulence level reduces the peak amplitude
of the wake loss and shifts the peak pitchwise towards the pressure side.
The current chapter will present how the problem was set up in the OpenFOAM
environment. In the first part it is shown how the mesh for solving the problem was
obtained and modified in order to be used in OpenFOAM and the second part shows how
the cases were defined and run in OpenFOAM.
3.1 Geometry and Mesh
As it could be seen from the previous section, the T106 blade is a well known test
case. The particular profile in the present study is the T106A which have a pitch of 0.799
chord lengths between blades, the specification can variate from T106A to T106D with
increasing pitch between blades. The airfoil is highly cambered and has rounded leading
and trailing edges. A turbine cascade is an aerodynamic device composed by a number
of blades placed at a radial distance from one another, and they are connected on a hub
like a fan. Since these blades have a high aspect ratio, they are normally simulated as
two dimensional blades positioned on top of one another. Experimental measurements
are normally carried on the middle blade of setups with five or seven blades. In numerical
simulations it is usual to see meshes with one blade in the middle of the domain and
periodical boundary conditions on top and bottom of the domain like in Reference [16]
and also domains with the pressure side of the blade on the top of the domain and the
suction side of the blade on the bottom of the domain like in Reference [15], the first
approach was also used in the current work.
The mesh employed to solve the problem was generated by a program developed within
the work done by Sandberg et al. [16], it is a high quality mesh designed for a finite
difference DNS solver and it was adapted in the current project to be solved within
a finite-volume methodology in OpenFOAM. The mesh was constructed based in the
methodology developed by Gross and Fasel [36] for turbine cascades by solving a Poisson
equation. It was conceived as a hybrid O-type mesh around the profile and an H-type
grid away from the profile. Due to the rounded leading and trailing edges of the blade,
the O-type grid will allow a good resolution in these regions and will ensure orthogonality
on the near wall cells around the profile. The H-type grid employed away from the profile
will allow the implementation of the periodic boundary conditions. The grid is composed
by nine blocks, and it is shown in Figure 3.1.
The O-type section is composed of the blocks 3, 4, 5 and 7 and the H-type section is
composed from the remaining blocks. Detail on the leading and trailling edges of the mesh
are shown in Figure 3.2. There are four points within the mesh where an intersection of
five domains occurs: the connection of blocks 1, 3, 5, 2, 6 and 5, 7, 8, 6, 9, shown in
Figure 3.3 and two of them due to the periodic boundary conditions on the top/bottom
connection, elements 1, 3, 4, 2, 6 and 4, 7, 8, 6, 9. According to Sandberg et al. [16] at
41. 3.1. GEOMETRY AND MESH 25
Figure 3.1: Combined O-type/H-type mesh from Reference [16] used in the current work.
these points, the cells cannot be orthogonal and a maximum angle of 72◦
was enforced
in order to improve the quality of the grid, these points were also moved away from the
blade to a region where a high accuracy is not essential.
For the DNS study the authors states that the grid refinement close to the wall had
to be sufficient to resolve the wall structures and that the mesh could be coarser away
from the wall, however, one of the objectives of their study was to investigate the effects
of the incoming turbulence on the boundary layer of the blade, then a fine mesh was set
upstream of the blade profile and in the passage between the blades in order to resolve the
incoming turbulence. To confirm that the mesh was adequate for their study they shown
that the ∆y+
on the suction side is bellow 1.4 and the flow is laminar in regions where
∆y+
> 1 with at least 30 points across the boundary layer. On the pressure side, most
of the surface is below ∆y+
= 1 except for the first point and close to the trailing edge
where the flow is also laminar. On their study, ∆x+
< 10 and ∆z+
< 11 were employed
which was deemed to be adequate.
The mesh for the current work was obtained from Sandberg et al. [16] as an ASCII
file with the coordinates of the points for each one of the blocks of the two-dimensional
mesh, initially it was expected that the OpenFOAM utility plot3dToFoam would be able
to read the mesh and extrude it in order to be used by the solver. The extrusion process
is necessary because, in OpenFOAM, all simulations have to be performed with tridimen-
sional meshes, in two-dimensional simulations the mesh must have one cell thickness and
the two new faces generated by the third dimension must be set with an empty boundary
condition.
A simple Fortran program was written to read the points from the nine ASCII files and
create a mesh in the Plot 3D format. The utility was executed, and the extruded mesh
was created perfectly, however, only the boundary conditions for the blade were set, and
a different path had to be undertaken.
Pointwise was the software chosen by Holohan [37] to generate meshes in his thesis
using OpenFOAM as a solver. The program has several grid generation utilities and also
is capable of generating meshes to specific solvers such as OpenFOAM. In the present
case, what was needed was a program that could extrude the mesh and set the boundary
conditions for the solver, which was accomplished with Pointwise.
The procedure executed with Pointwise was to import the mesh in Plot 3D format,
then execute an extrusion, which was made with the command Create/Extrude/Translate
and a translation of one unit of length is performed in the z direction. The following step
was the execution of the command CAE/Set Boundary Conditions to set the boundary
42. 26 CHAPTER 3. THE PROBLEM
(a) Leading edge
(b) Trailing edge
Figure 3.2: Details of the leading and trailing edges of the mesh of the T106 blade.
(a) Point of connection of blocks 1, 3, 5, 2, 6 (b) Point of connection of blocks 5, 7, 8, 6, 9
Figure 3.3: Details of the mesh on the connection points of five different blocks.
43. 3.1. GEOMETRY AND MESH 27
conditions to the mesh: as it was mentioned earlier, the lateral boundaries are defined
as empty boundary condition; the profile was defined as wall boundary condition and
the other boundaries were defined as patch boundary condition1
. The mesh was then
exported to the OpenFOAM format with the command File/Export/CAE, and the five
files that compose the mesh in an OpenFOAM case were created.
OpenFoam meshes are defined by a hierarchical set of files that organizes the cell
distribution and it is composed by at least five different files:
• the points file is a list with the coordinates of all points in the mesh;
• the faces file is a list of all the mesh faces composed by the points of the previous
file;
• the owner file is a list of the number of the volumes that own the faces defined in
the previous file;
• the neighbor file is a list of the neighbor faces and
• the boundary file defines the boundary conditions for the mesh, this is the file where
the periodic boundary condition has to be defined.
The final step to get a working mesh in OpenFOAM environment was to set the
periodic boundary conditions on the top and bottom parts of the mesh, for that operation
OpenFOAM’s utility createPatch had to be executed, it uses the information from the
dictionary file createPatchDict that determines which boundaries are periodic and which
are the neighbors of the periodic boundaries. It is very important to make sure that the
point coordinates of the mesh on one of the periodic boundaries matches the correspondent
coordinates of the points on the other.
The original mesh was developed to DNS calculations, therefore, it is was expected to
be more refined than necessary for RANS simulations. The number of points in each of its
component blocks, number of cells and number of faces is presented in Table 3.1. During
the initial test simulations with the mesh in a two-dimensional configuration, the time
of execution of the iterations was considered short enough to carry on with the studies,
with some of the simulations reaching convergence in less than five hours. However it was
thought that a comparison of the results with a less refined mesh could also bring new
information about simulation times and the quality of the results obtained.
A less refined mesh was created based on the original mesh, since the original mesh
was obtained in ASCII format with the cartesian points of the mesh elements, the idea of
eliminating some of the intermediate points of the mesh came to mind. A simple program
in Visual Basic within Microsoft Excel environment was made in order to select the x
and y coordinates correspondent to a specific point and erase it. The refinement of the
mesh in the direction normal to the wall was kept the same as the original mesh, and the
points in the direction tangential to the wall were reduced in its half as shown in detail
on Figure 3.4.
The number of points in each direction of all meshes was even, then, to keep the size of
each of the nine blocks the same, the first and the last column of elements were maintained
and the intermediate columns were eliminated alternately until the last column that was
maintained to keep the size of the mesh. The neighbor of the last column was eliminated,
as shown in Figure 3.5, this process created a column with a wider thickness, in order to
1
In OpenFOAM is a list of boundary faces is called a patch, in the current work each patch will be
associated to a distinct boundary
44. 28 CHAPTER 3. THE PROBLEM
(a) Original Mesh (b) Coarse Mesh
Figure 3.4: Details of the original mesh and the coarser mesh over the suction side of the
T106 blade.
Table 3.1: Number of elements in each of the two meshes used in the study
Element Original Mesh Coarse Mesh
Block 1 288 x 192 144 x 96
Block 2 288 x 48 144 x 48
Block 3 144 x 192 144 x 96
Block 4 144 x 240 144 x 120
Block 5 144 x 240 144 x 120
Block 6 48 x 240 48 x 120
Block 7 144 x 192 144 x 96
Block 8 288 x 192 144 x 96
Block 9 288 x 48 144 x 48
Number of points 555,612 216,340
Number of cells 270,825 107,409
Number of faces 1,084,718 430,397
avoid the problem in critical regions of the mesh, whenever possible these wider elements
were positioned close to the external boundaries of the mesh.
Special care was taken in the mesh intersections, since a previous mesh presented
numerical instabilities on these points, nevertheless, in the central blocks 4, 5 and 6 it
was impossible to avoid a wider element in the connection of the blocks, the detail of the
intersection points of the mesh is shown on Figure 3.6, in the left branch it is possible to
see the right-hand side blocks with the wider element in the connection of mesh blocks.
In the H-type blocks 1 and 8 the reduction of the number of cells had to be made
both in the horizontal direction and in vertical direction, because the number of vertical
elements on these blocks defines the number of elements on the wall direction in blocks 3
and 7. A detail of the leading and trailing edges on blocks 3 and 7 are shown in Figure
3.7. The total number of points in each block and the total number of cells and faces for
the modified and coarser mesh are also presented in Table 3.1, the total number of cells
was reduced in almost 60% when comparing with the original mesh.
A tri-dimensional view of the mesh is shown in Figure 3.8, the lateral faces were hidden
to allow a better visualization of the boundaries (patches) and their name convention, it
also shows the coordinate convention used when solving the numerical problem.
45. 3.1. GEOMETRY AND MESH 29
(a) Original Mesh (b) Coarse Mesh
Figure 3.5: Detail of the technique adopted do eliminate points to generate a coarser
mesh.
(a) Connection of blocks 1,3,5, 2 and 6 (b) Connection of blocks 5, 7, 8, 6 and 9
Figure 3.6: Details of the connection of blocks of the coarse mesh of the T106 blade.
46. 30 CHAPTER 3. THE PROBLEM
(a) Leading edge
(b) Trailing edge
Figure 3.7: Details of the leading and trailing edge on the coarse mesh of the T106 blade.
Figure 3.8: Name convention for the boundaries of the mesh used in the current work
