Internship_Report_Mazza (2)

Department of Mechanical Engineering
TURBULENT NON PREMIXED
FLAME MODELLING USING
FLAMELET-GENERATED MANIFOLD
IN OPENFOAM 2.1.1.
Marco Mazza
February 8, 2016
IN OPENFOAM 2.1.1.
Marco Mazza
February 8, 2016
IN OPENFOAM 2.1.1.
Marco Mazza
February 8, 2016
IN OPENFOAM 2.1.1.
Marco Mazza
February 8, 2016
IN OPENFOAM 2.1.1.
Marco Mazza
February 8, 2016
IN OPENFOAM 2.1.1.
Marco Mazza
February 8, 2016
IN OPENFOAM 2.1.1.
Marco Mazza
February 8, 2016
IN OPENFOAM 2.1.1.
Marco Mazza
February 8, 2016
IN OPENFOAM 2.1.1.
Marco Mazza
February 8, 2016

Contents
1 Introduction 2
2 Theory 4
2.1 The FGM method . . . . . . . . . . . . . . . . . . . . . . . . . . 4
2.1.1 Inclusion of Mixture fraction . . . . . . . . . . . . . . . . 5
2.1.2 Manifold structure and implementation . . . . . . . . . . 6
2.2 Turbulent flows . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7
2.2.1 The k-epsilon model . . . . . . . . . . . . . . . . . . . . . 8
2.3 Numerical schemes . . . . . . . . . . . . . . . . . . . . . . . . . . 10
2.3.1 The SIMPLE algorithm . . . . . . . . . . . . . . . . . . . 10
2.3.2 The SIMPLE method in OpenFoam . . . . . . . . . . . . 12
2.3.3 The PIMPLE algorithm - a variation of the SIMPLE pro-
cedure . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14
3 Results 15
3.1 Simulation Setup . . . . . . . . . . . . . . . . . . . . . . . . . . . 15
3.1.1 Geometry and mesh . . . . . . . . . . . . . . . . . . . . . 16
3.1.2 Boundary conditions . . . . . . . . . . . . . . . . . . . . . 17
3.2 Cold flow results . . . . . . . . . . . . . . . . . . . . . . . . . . . 19
3.3 1D Manifold- Cold flow . . . . . . . . . . . . . . . . . . . . . . . 22
3.4 2D Manifold . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 23
3.4.1 Combustion inclusion . . . . . . . . . . . . . . . . . . . . 25
3.4.2 Analysis of temperature results . . . . . . . . . . . . . . . 27
4 Conclusions 31
Appendices . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 32
1

Chapter 1
Introduction
The present work has been carried out within the framework of the European
initiative of the Dreamcode project. At the moment different institutions are
collaborating to develop state of art technologies which can improve the en-
vironmental performances of airplanes and air transport. At the TU/e the
Combustion Technology group is currently working on laminar and turbulent
combustion modelling.
More specifically, the research is focusing on reduced chemistry modelling
and application of flamelet generated manifolds method (FGM). Through those
research methods quantitative analyses of different pollutants emissions are
made available. It is therefore possible to outline, for specific case studies,
the rate of production of specific pollutants such NOx, CO2, CO, soot or soot
precursors.
This study aims to investigate the theory behind those models as well as
to inspect them through computational simulations. In particular, OpenFoam
2.1.1 is used as main computational fluid dynamics tool. A non premixed tur-
bulent jet flame is investigated; the case study provided by the University of
Adelaide, Australia, is employed to construct a model in OpenFoam which in-
tends to recreate the physical phenomena involved in the combustion process.
The problem is approached through discrete steps of increasing complex-
ity. Firstly, a theoretical description of the method is presented in Chapter 1.
Thereon, from Chapter 2 the results are presented. Initially, a RANS model
is used to represent the turbulence of non reacting flows. At this point the
focus is on understanding to which extent the gaseous species travel and dif-
fuse reciprocally into each other. Afterwards, mixture fraction is included as a
scalar quantity transported by the flow; this change has no influence on flow
patterns since mixture fraction is included as a passive scalar quantity. The
lookup procedure based on Flamelet Generated Manifolds method is included
subsequently. Originally a 1D manifold is used to evaluate the local redistribu-
tion of density due to mixing by means of a time dependent RANS simulation.
Combustion is then introduced in the following stage, enriching the manifold
with a further controlling variable. The obtained results are finally compared
2

with the experimental data, oﬀering an opportunity to highlight strengths and
weaknesses of this research.
3

Chapter 2
Theory
The following chapter provides insight into the scientific foundations above
which this investigation lays; the theoretical preliminaries involve the descrip-
tion of the FGM method, the characterization of turbulent flows as well as a
short overview of the recurring numerical methods.
2.1 The FGM method
Flamelet Generated Manifolds is a chemistry reduction method which shares the
approach of flamelet models and other reductions techniques based on chemical
steady-state assumptions. From the flamelet model emerges the idea of repre-
senting multidimensional flames through a formation of one dimensional flames
(flamelets) enclosed by the flow field. The FGM method was firstly described by
van Oijen [18], to which this study refers to. In the FGM technique the progress
of a certain reaction is construed in terms of few control variables, for which
the solutions of the transport equations are found with the assistance of a CFD
solver. The reaction progress variables can be defined as any linear combination
of species mass fraction which guarantees Y > 0 [3]. In a premixed flame
it ranges between Yu (unburned mixture) and Yb (burned mixture). Theoreti-
cally any species or combination of species can be chosen, as long as Y shows a
monotonic profile in the whole interval between the unburned mixture and the
chemical equilibrium.
During the pre-processing stage the flamelet equations are solved and the
solutions stored into the so called manifold. In this database, obtained for given
initial conditions, the thermochemical variables describing the combustion are
parametrized by the controlling variables. This is realised once for a given
mixture and, eventually, the results can be used in a series of simulations.
At the Eindhoven Univerisity of Technology, the Chem1d software is suc-
cessfully employed in the pre-processing stage in order to solve the flamelets
equations. This set of equations is deduced from the conservation equations
with the aid of the kinematic equation and the stretch rate equation. For the
4

sake of simplicity only the final group of equations is listed, the complete deriva-
tion can be found in [18].
The flamelet equations are used to determine the mass burning rate m, the
flux of species mass fraction Fi and the flux of enthalpy Fh, which are key
parameters for flame front structure modelling. The parameter s is introduced
as the arc length perpendicular to the flame surface. The introduction of s is
necessary to adjust the set of formulas in a flame adaptive form, referred to
as the quasi 1D form. Neglecting all discrepancies and perturbations from the
one dimensional flame behaviour, the flamelet ensemble of equations is finally
casted as follow:
∂m
∂s
= 0 (2.1)
∂mYi
∂s
−
∂
∂s
λ
∂Leicp
∂Yi
∂s
= ˙wl i ∈ [1, Ns] (2.2)
∂mh
∂s
−
∂
∂s
λ
cp
∂h
∂s
−
∂
∂s
λ
cp
Ns
i=1
1
∂Lei
− 1 hi
∂Yi
∂s
= 0 (2.3)
Where Le is the Lewis number, λ is the thermal conductivity and Cp the spe-
cific heat. The Lewis number is defined as the ratio between thermal diffusivity
and species mass diffusivity.
Lei =
λ
ρDicp
(2.4)
Crucially the FGM approach has gained importance over the last years for
its accuracy and simplicity, being preferred to other methods that deal with the
inherent stiffness of governing equations by means of large data-structures.
2.1.1 Inclusion of Mixture fraction
The initial stage of the cold flow simulation is devoted to solve the velocity
field, then, the mixture fraction is introduced as a passive scalar transported
by the flow. In the literature, for two-phase mixtures, the mixture fraction Z is
adequately estimated through the following formula [12]
Z =
sYF − Yox + Yox,2
sYF,1 + Yox,2
(2.5)
being YF,1 the fuel mass fraction in stream 1, Yox,2 the oxidiser mass frac-
tion in stream 2 as well as s is the stoichiometric ratio. The mixture fraction
is remarkably useful in providing insight to the level of mixing between oxidiser
and fuel, which in turn determine the position of the flame in non-premixed
cases [12]. Considering the iso-plane YF = sYox one could obtain a detail map-
ping of several thermophysical parameters, since, fore reactive flows, this is the
5

surface where the combustion process is more efficient, leading to temperature
and chemical reaction rate peak values. Furthermore, this parameter as well
as pressure and enthalpy are conserved variables in combustion processes [18],
meaning that the mixture fraction field found for the converged solution can
be fruitfully employed to initialise the domain in the later simulations, where
combustion is included. The aforementioned equation can be characterised as
follows [18]:
∂ρZ
∂t
+ · (ρUZ) = · (D Z) (2.6)
The first term is the unsteady term, which is neglected in the steady solvers,
the second term, namely the divergence of velocity and mixture fraction, corre-
sponds to the convection term whereas the right hand side terms is the diffusion
term. The laplacian Z regulates the magnitude of the diffusion. Moreover,
the diffusion coefficient D is defined as the sum of two terms: a laminar com-
ponent and a turbulent component. The laminar part is tabulated assuming
the average diffusion coefficient of gaseous species in air, the turbulent part is
tuned by means of the Schmidt number which is defined as the ratio between the
viscous diffusion rate and the mass diffusion rate. In combustion modelling this
parameter is usually set to 0,7 although smaller values are not seldom used [9].
In this study the turbulent diffusivity as 0.7−1
µt.
2.1.2 Manifold structure and implementation
The implementation of FGM in a reacting flow can be considered as a sequence
of two steps: the initial step exists of the generation and storage of the flamelet
data and the second stage is the coupling of a FGM with a multi-dimensional
combustion computation, here performed with the software OpenFoam 2.1.1.
The FGM database is obtained for a given mixture, which in this case resembles
the mixture employed at the University of Adelaide to evaluate the performance
of the burner [20]. As a consequence of that, the fuel composition by mass is
determined by 63.8% C2H4, 4.6% H2 and 31.6% N2 as well as the temperature
for fuel and coflow is set equal to 294 K. To generate the manifold a specific
chemistry model has to be considered: in this case the diffusion counterflow
flamelets model was used. Furthermore, the mixture averaged model is used to
account for the species transport. In the mixture averaged model the diffusion
coefficient of a single chemical species is found as follows [6]:
Di,m =
(1 − wi)
xk
Di,k
(2.7)
Where wi is the mass fraction of component i, xk the mole fraction of com-
ponent k, Di,m the diffusivity coefficient of the component i in the mixture and
Di,k the diffusivity coefficient of the component i in the component k. As it is
6

possible to see, the diffusivity of a certain species into the mixture is obtained
averaging the diffusivity in all the chemical species involved in the reaction. As
it is expected, the diffusion coefficients obtained are different for every chemi-
cal species, which makes this method suitable for non premixed flames where
preferential diffusion effects play an important role.
The calculation in Chem1D, the in house tool employed to compute one di-
mensional flames, is performed solving the flamelet equations (2.1)-(2.3). The
importance of those equations can be understood recalling how the evolution
of all the species mass fractions Yi is casted in the flamelet equations. Hence,
the progress variable Y is defined starting as a linear combination of different
species mass fractions. Flamelet solutions are as such mapped as a function
of Y, in such a way that every thermochemical variable φ is directly described
as φ=φ(Y) [18]. Finally, the cfd solver evaluates the transport equations for
the controlling variable. The manifold is usually stored in a tabulated form, in
such a way that the boundaries of the thermophysical variables can be identi-
fied promptly. Importantly, in Chem1D is also possible to define a non-uniform
gridpoint distribution, increasing the sensitivity of the progress variable only for
a limited range of values. This can be done tuning the grid-power factor, which
contributes to save computational resources reducing the data storage by means
of grid selective refinement. This is undoubtedly an interesting feature consid-
ering, for instance, how around the flame front a wide range of thermophysical
parameters (e.g. temperature, CO2 mass fraction) withstands sharp increases
within an infinitesimal distance. The manifold is parametrized by a progress
variable as well as a controlling variable, in this case the mixture fraction. The
transport equation for the progress variable is similar to Eqn 2.6. for mixture
fraction:
∂ρY
∂t
+ · (ρUY) = · (D Y) (2.8)
Theoretically, it is also possible to introduce an additional controlling vari-
able when it is expected that its variation would introduce significant modifi-
cations to the computational model, however, in that case the gain in term of
detail enhancement would be reduced or negated entirely by the intensification
of computational time.
2.2 Turbulent flows
In fluid dynamics, turbulent flow is a flow regime characterized by chaotic prop-
erty changes. This includes low momentum diffusion, high momentum convec-
tion, and rapid variation of pressure and flow velocity in space and time. The
transition from laminar to turbulent flow occurs when inertial forces acting on
the fluid overtake the viscous forces; mathematically the magnitude of the two
forces are compared through the Reynolds number. This parameter is defined
as ρV D/µ where ρ is the gas density, V the velocity, D the characteristic length
7

and µ the dynamic viscosity. The general rule involves turbulent flows to start
from Re = 4000, whereas the transition region ranges between Re = 4000 and
Re = 2000 and the laminar flow develops when Re is below 2000 [10].
From an engineering perspective, turbulence is a stochastic phenomenon
which can be statistically described by the mean and variance of quantities.
Flow velocities can dicotomically be split into a mean part and a fluctuating
part, by means of Reynolds decomposition:
U(x, t) = U(x, t) + u(x, t) (2.9)
The literature usually distinguishes between turbulent flow simulation and
models [17]. In the first case equations are solved for a time dependent ve-
locity field that, to some extent, represent the velocity field U = U(x, t). In
contrast, in a turbulence model, equations are solved for some mean quantities,
for example U(x, t) and ε. The first category includes the DNS approach,
which is computationally extremely expensive although allows to resolve all
the turbulence scales, and the LES method. With the Large Eddy Simulation
method the unsteadiness of turbulence is partially resolved, however the process
is again cpu-demanding. An example of turbulence model is the Reynolds aver-
aged Navier-Stokes (RANS) model, which involves the solution of the Reynolds
equations to determine the mean velocity field (U). In RANS the turbulent vis-
cosity is a crucial parameter since it is used to model the Reynolds stresses; it
can be obtained from an algebraic relation (such as in the mixing-length model)
or from scalar quantities such as κ and ε for which modelled transport equations
are solved [17].
2.2.1 The k-epsilon model
The RANS approach involves filtering in time, implying that for the velocity
field time averaged mean values are estimated. Firstly, the continuity equation
as well as the Reynolds equations for mean momentum in a 3D configuration
can be introduced as follows [17]:
· U = 0 (2.10)
ρ
D Uj
Dt
=
∂
∂xi
µ
∂ Uj
∂xj
+
∂ Ui
∂xi
− P δij − ρ UjUi (2.11)
where µ
∂ Uj
∂xj
+ ∂ Ui
∂xi
is the viscous stress, P δij is the isotropic stress from
the mean pressure field and ρ UiUj is the Reynolds stress from the fluctuating
velocity. Together with the three components of the Reynolds equation, the
Poisson equation for pressure is available:
8

2
P = −ρ
∂Ui
∂xj
∂Uj
∂xi
(2.12)
The equation is obtained for incompressible flows performing the divergence
of the momentum equation. This is a consequence of incompressibility acting
as a constraint for the pressure. However, at these conditions the problem is
undetermined since, including the Reynolds stresses, there are more than four
unknowns. Thus, two new variables are introduced, namely κ and ε. κ is defined
as the turbulent kinetic energy and it is determined starting from the velocity
components though the following relation:
k =
1
2
UiUj (2.13)
Similarly, ε measures the turbulent kinetic energy dissipation rate; the good
practice involves the usage of empirical formulas to deal with this parameter,
the following refers to a flow in conduct [1] [19] [3].
ε = 0.164
k2
l
(2.14)
Where l is the characteristic length and κ the aforementioned turbulent
kinetic energy. The calculation of the turbulence parameter for boundary fields
will be dealt in more detail in the Results chapter. The closure is obtained
casting the turbulent viscosity as a function of these two new variables:
µt = 0.09
k2
ε
(2.15)
The problem is now determined since the turbulent viscosity hypothesis,
which is part of the k epsilon model, states that the Reynolds stresses de-
pends on turbulent viscosity. Knowing the turbulent viscosity field the reynolds
stresses can be quantified accordingly, in such a way providing the closure to
the Reynolds equations. Therefore, the two transport equations for κ and ε
permit to determine the distribution of these variables for the entire flow field,
providing an elegant solution to the problem. The two balance equations are
casted as follows:
Dk
Dt
=
∂
∂xi
µ +
µt
σk
∂k
∂xi
+ Pk − ε (2.16)
Dε
Dt
=
∂
∂xi
µ +
µt
σε
∂ε
∂xi
+ Cε1
ε
k
Pk − Cε2
ε2
k
(2.17)
9

Where Pk is the source term, which depends on the velocity components,
and the other model constants are usually set according to Launder and Sharma
(1978) [5]:
Cu = 0.09; σk = 1.0; σε = 1.3; Cε1 = 1.44; Cε2 = 1.92
The main downside of this two equations model relies on the strong assump-
tions needed to obtain the balance equations for k and epsilon. These involves
homogeneous and isotropic turbulence and importantly high Reynolds number.
2.3 Numerical schemes
For what concerns the choice of the discretization scheme the approach of Ver-
steeg and Malaskeera [19] has been followed. For convection-diffusion problems,
such as this case study, the best practice involves the estimation of the cell
Pecklet number in order to account for the relative strengths of convection and
diffusion. Considering the flow characteristic this parameter is expected to reach
high values as a consequence of the dominance of convection on diffusion. Conse-
quently, an Upwind discretization scheme has been adopted, ensuring that the
transportiveness property of the fluid flow is conserved in the computational
model. Transportivness is a characteristic of a fluid in motion for which the
properties of a certain fluid particle are influenced by alternatively the upstream
or downstream condition, depending on the flow direction of influence [13]. A
central differencing scheme, which employs interpolation of transport proprieties
to cell face, averages the proprieties at a certain grid point without distinguish
between the different influence of points located upstream or downstream with
respect to the direction from which the advective flow emanates. This is accept-
able when the Pecklet number approaches zero, however, the numerical errors
increase at high Pecklet number where the thermopyshical proprieties at the
grid points originate from asymmetric contributions. The upwind differencing
schemes, which treats the diffusion term in the discretized convection-diffusion
equation equally to the central differencing scheme, estimates the convection
term in the aforementioned equation as the difference between two contributes.
The first one is a function of the mass flux calculated at the nodal point of
interest whereas the second one is the mass flux estimated at the nodal point
of preceding cell with respect to the flow direction [19]. To conclude, the Up-
wind differencing scheme is often preferred to the central differencing scheme,
however, a drawback of such a choice arises when considering that the former
is a first-order scheme in space whereas the latter is a second-order scheme in
space [14]. Thus, in the first case, if the cells size becomes half the errors be-
comes roughly half accordingly. With central differencing scheme the same cell
refinement would minimize the error by a factor four.
2.3.1 The SIMPLE algorithm
The present description aims to shed light on one of the most widely used algo-
rithm in computational fluid dynamics, the SIMPLE algorithm, which acronym
10

Figure 2.1: Grid overview [14] Figure 2.2: Cell faces and interfaces [14]
stands for Semi-Implicit Method for Pressure-Linked Equations. Its relevance in
this study relies on the centrality of this procedure in the simpleFoam solver, an
OpenFoam steady-solver for incompressible turbulent flows which is employed in
the non reactive flows simulation. The SIMPLE approach involves the coupling
of the Naviers-Stokes equation with an iterative procedure, which is summarised
below. Firstly, it is necessary to introduce the discretised form of the Navier-
Stokes equation for a staggered grid. The construction of a staggered grid is
successfully employed in rendering the correct pressure distribution, this in turn
avoids mistakes in momentum prediction.
Figure 2.1 can be observed to have a better understanding: let us assume
that it is interesting to know the pressure gradient value at the nodal point P,
to perform this estimation the values of P at the cell boundaries ”w” and ”e”
need to be determined. Since the pressure value in P is known, at the interfaces
the values can be calculated by means of linear interpolation:
∂p
∂x
=
pe − pw
δx
=
pE +pP
2 − pP +pW
2
δx
=
pE − pW
2δx
(2.18)
where δx corresponds to the cell width. As can be seen, according to Figure
2.2 unity pressure values can substitute PE and PW , yielding a zero discretised
pressure gradient. This finding does not appear to support the obviousness that
the pressure exhibits spatial oscillations in both directions [19, p. 137]. Thus,
defining the velocity at the grid points would introduce a miscalculation in
the discretised momentum equation, due to the fallacious pressure estimation.
The problem can be solved introducing a staggered grid, where the location of
scalar quantities such as density or pressure is split from the location of vector
quantities such as velocity. The former are defined at the grid points whereas the
latter are defined at the cells faces. In this way the pressure gradient results in
the correct momentum source term. At this point, following the procedure of H.
Veersteeg and H. Malalasekera [19], the discretised momentum equation for the
horizontal direction in the staggered grid coordinate system can be introduced:
aP,uuP =
nb
anb,uunb − (pP − pW )AW,u + Su u V (2.19)
11

where Aw,u is the cross-sectional area through which the mass flux is calcu-
lated, uV the cell volume as well as Su is the source term of the momentum
equation deprived of the pressure gradient. The term aPu
and the summation
nb
anb,uunb, which vary across the differencing methods (upwind, central), re-
sult from the discretisation procedure and capture the convective flux as well as
the diffusive conductance through the cell faces. For the sake of simplicity only
the equation for the horizontal component of the velocity is listed, however, the
equation for the vertical component would be analogue. Hence, velocity and
pressure are then divided into two components: an initial guess as well as a
correction term.
u = u + u (2.20)
p = p + p (2.21)
Substituting the pressure guess p into Eqn. (2.19) and then subtracting it
from the same equation the discretised momentum equations as a function of
the pressure correction term is casted. During the calculation the source term
Su cancels out, moreover,
nb
anb,uunb can be neglected considering that for a
converged solution those terms are null [16]. As a result, the velocity correction
equation is found:
up = −
(pP − pW ) AW,u
aP,u
(2.22)
Introducing this equation, together with Eqn. (2.20), into the discretised
continuity equation (e.g. the discrete flux balance for the finite volume) the
pressure correction is found. Consequently, the total pressure can be calculated
with Eqn. (2.21), then, through Eqn. (2.19), the new pressure field is used
to recalculate the velocity field. Finally, if convergence is achieved for all the
considered variables the loop is stopped, otherwise a new iteration is started
replacing u with the final value of u [16].
2.3.2 The SIMPLE method in OpenFoam
As it was already mentioned, the simple algorithm is implemented in OpenFoam
in the simpleFoam solver, for which there is a justified interest as it is a steady
solver for incompressible, turbulent flows. The following paragraph outlines the
steps followed to introduce the simple algorithm into simpleFoam, focusing on
the related part of the software code. When accessing the solver main direc-
tory three important libraries can be found: the simpleFoam.c file, the Ueqn.H
file as well as the pEqn.H file. The solver structure is intertwined with an ex-
tensive number of libraries and subdirectories, however, the implementation of
12

the simple algorithm relies nearly entirely on these three elements. Observing
the simpleFoam.c file one could observe the file headers, where the geometry is
created, the boundary conditions set as well as the turbulence model specified;
hence, the iteration loop starts including the UEqn.H as well as the pEqn.H file.
The former is also called momentum predictor since it contains the instruction
for the calculation of the discretised Navier Stokes equation, the latter contains
pressure and velocity correction routines. The momentum equation is shaped
as follows:
· (uu) = −
1
ρ
p + ν 2
u (2.23)
Initially, The velocity field is predicted in the UEqn.H file. As can be no-
ticed, there are specific parts of the code referring to each of the three terms
listed in the Navier Stokes equation, namely the conductive term, the pressure
gradient term as well as the diffusion term. Thus, the convective term · (uu)
is indicated in the code by the syntax fvm :: div(phi, U) whereas the diffusion
term ν 2
u is called by the keyword turbulence− > divDevReff(U) [11]. The
diffusion term is also the member of the Navier Stokes equation influenced by
turbulence, in fact, as it is shown in the RASmodel.H library, compared to the
laminar model the viscosity is substituted by the effective viscosity that is rep-
resented by the sum of two components: the laminar viscosity, which can be
assumed as standard air viscosity, and the turbulent viscosity, which is calcu-
lated from k and epsilon through Eqn. (2.15) [11]. The velocity field can be
calculated by means of an initial guess of the pressure, visible in the RHS of
the equation solve (UEqn() = −fvc :: grad(p)) [2], implying that for the first
iteration the initial internal field (specified in the boundary conditions folder) is
used. The LHS of the equation contains the aforementioned terms for convec-
tion and diffusion. At this point the pEqn.H file is accessed; here we can find the
velocity correction equation based on Eqn. (2.22). Initially, aP , u is calculated,
then the resulting coefficients are introdced into the velocity correction term to
adjust the velocity. The operation is accomplished by means of two statements:
volScalarFieldrAU(1.0/UEqn().A()) is responsible for the creation of the ma-
trix defining aP , u in each cell whereas U = rAU ∗ UEqn().H() is the velocity
correction term [2].
Once the first valuation of the velocity field is known, the pressure is calcu-
lated through the following equation [2]:
·
1
aP
p = · (UAcell) (2.24)
as indicated by the line fvm :: laplacian(1.0/AU, p) == fvc :: div(phi).
UAcell represents the volumetric flux. Hence, in the final stage the velocity is
updated considering the new pressure value. Velocity and pressure are linked
together through the command U− = rAU ∗ fvc :: grad(p), in other words
imposing
13

U = −
1
aP
P (2.25)
Finally, the volumetric flux phi is corrected; the simulation stops if the
convergence criteria are satisfied otherwise the loop is repeated. For further
details the reader can refer to [8].
2.3.3 The PIMPLE algorithm - a variation of the SIMPLE
procedure
As explained in the previous section, SimpleFoam is an OpenFoam solver dedi-
cated to steady simulations for laminar as well as turbulent flows. In comparison
with transient solvers, the attractive feature of such a solver relies on the re-
duced computational resources required to complete a simulation. However,
this is achieved excluding the time dependent terms in the set of equations
considered, thus, ensuring that the final solution is converged in space but not
necessarily in time. The counterpart of the SimpleFoam which also considers
variations in time is the PisoFoam solver, in with is also possible to apply the
momentum corrector multiple times. The rate at which the simulation can ad-
vance in time is tuned setting a proper value for the time steps which result in
a unique value of the Courant number. In a two-dimensional problem this last
parameter is defined as:
C =
ux t
x
+
uy t
y
(2.26)
where ux and uy are the velocity components, x and y the lengths mea-
suring the cells edges and t is the time step. This parameter, which describes
the fluid motion, is usually kept below the unity value. In fact, in the other case
a fluid particles crosses more than one cell within a time step, affecting the con-
vergence negatively. In case of a complex geometry it would be straightforward
to reduce the time step to save computational time, however, this interven-
tion is limited by the fact that the Courant number can only increase to a
limited extent. To overtake this problem the Pimple algorithm has been intro-
duced; in particular the PimpleFoam solver has the traditional characteristics
of unsteady solvers enhanced with the ability of exploiting relaxations factors,
which is a peculiarity of steady solvers. The procedure is controlled through
the commands nCorrectors and nOuterCorrectors, the former recalculate the
momentum starting from the modified pressure value, which is obtained from
Eqn. 2.31, the latter recalculate pressure from the updated value of the veloc-
ity, which is found with Eqn. 2.22. In this way each time step is enriched with
subsequent correctors loop where relaxation factors are applied. Through the
relaxation factors the convergence in space is found gradually; finally, when the
values of the residuals are below the specified limit, the loop is interrupted and
the simulations steps in time towards the final solution.
14

Chapter 3
Results
3.1 Simulation Setup
Before diving into the physical aspects of the simulation it is necessary to discuss
shortly the main features of the so called pre-processing stage. In cfd pre-
processing involves two different tasks: definition of the geometry and grid
generation. Defining a suitable geometry for the problem considered implies the
creation of a computational domain where ordinary and differential equations
can be solved, returning a solution which is usually a set of physical or chemical
parameters. Once the boundaries of the model are set, the domain is divided
into a number of smaller, non overlapping sub-domains which constitutes a
grid of cells [19]. The set of physical parameters describing a particular flow is
defined at the core of each cell, therefore, the solution of the physical problem in
continuous space is approximated by a solution in discrete gridpoints. It follows
that, after the discretization, the accuracy of the solution is governed by the
number of cells in the grid. A high number of points would affect positively the
accuracy of the output as well as it would increase the computational cost and
the simulation time. A smart way to achieve great definition without incurring
in the aforementioned pitfalls consist in adopting a non-uniform mesh: the grid
is selectively refined in such a way that the detail is enhanced only where large
variations occur from point to point. With respect to the cells shape a wide
range of options is available, ranging from tetrahedral to hexahedral. Three
parameters are used to evaluate if the choice is appropriate or not: the skewness,
which indicates the distortion caused by the difference of angle amplitudes,
should be minimised, the smoothness, which accounts for the cells dimension
graduation, should be guaranteed as well as the aspect ratio, which is the ratio
between the longest to the shortest side of a cell, should approach the unity
value [15].
15

Figure 3.1: Experimental setup
Figure 3.2: Axial symmetric
domain [1]
3.1.1 Geometry and mesh
In this case study, considering the radial symmetry of the experimental setup,
a 2D axi-symmetric domain has been modelled. Avoiding the implementation
of a three dimensional domain results in reduced computational time, however,
it should not be forgotten that the physical description of the problem is nega-
tively affected. This can be understood considering, for instance, the asymmet-
ric distribution of turbulent structures, e.g. eddies in swirling flows, under high
Reynolds number conditions. Hence, although not entirely acceptable, this sim-
plification can be fruitfully employed in RANS simulations, in which averaged
thermophysical parameters are considered.
The original experimental set-up is shown in Figure 3.1, as can be seen the
fuel jet, which is supplied by the central burner, is surrounded by air coming
from a square pipe. In the picture, for the sake of clarity and simplicity, the fuel
pipe diameter is exaggerated and the fuel duct thickness (1 mm) is neglected.
Starting from this configuration a similar geometry was created in OpenFoam;
radially, in order to save computational resources, the domain is contracted to
a 35 mm width, being this amplitude large enough to allow a comparison with
the experimental results available in radial direction.
In OpenFoam the computational domain is necessarily defined in a three
dimensional space, however, under particular impositions one dimension can
be neglected during the calculation, leading to a two-dimensional problem. The
methodology is outlined in the following section: firstly a wedge is defined, if the
central angle is smaller than 5◦
only two dimensions will be considered, namely
the direction coincident with the symmetry axis as well as the one bisecting the
central angle. Furthermore, particular care must be taken when defining each
boundary of the domain. In particular, in order to reproduce a two dimensional
axi-symmetric case the lateral faces of the domain need to be assigned with the
type of surface called wedge. In this way OpenFoam considers the domain as
created from the rotation of the two lateral planes; looking at Figure 3.2, the
wedge type faces are ACDF and CBEF respectively. The creation of a 2D
axi-symmetric geometry is completed assigning the empty type surface to the
region, or more precisely the segment, CF. As a consequence of that, in the
azimuth angle direction, no solution is required.
16

Regarding the mesh, a hexahedral grid has been employed. As it is shown
in Figure 3.4, the area of the domain surrounding the inlet is refined in such
a way that the aspect ratio approaches the unity value for the cells along the
interface fuel/air. To serve this purpose expansion ratios equal to 4 are imposed
in the radial and axial direction. The expansion ratio is used to define the ratio
between the length of the start cell to the end cell with respect to a certain
direction. Figure 3.5 helps to clarify the refinement strategy employed for the
inlet plane. As can be seen, 50 cells span the radial direction; the smaller
cell, placed at the fuel side, has a width of 0,3 mm whereas the end cell is 1.2
mm large. In this way the detail is enriched in the region of more interest,
namely where the fuel is injected. The thickness of the wedge is determined
imposing a central angle of 4◦
, which results in a width of 2,44 mm. Finally,
Figure 3.3 outlines the grid distribution in the entire domain; the vertical axis
corresponds to the axial direction whereas the horizontal axis corresponds to
the radial direction. The height of the domain is set equal to 0,2 m, the width
in radial direction, as already mentioned, is 0.035 m.
Figure 3.3: Mesh structure
Figure 3.4: Inlet grid refinement
Figure 3.5: Inlet surface (mesh in
black) and unresolved surface (mesh
in dark blue)
3.1.2 Boundary conditions
When solving differential equations appropriate boundary conditions need to be
applied. Those are key components of the mathematical and physical model,
since the motion of flow as well as the magnitude of energy, momentum and
mass fluxes into the computational domain are tuned considering the values
17

imposed at the boundaries. In cfd the boundary surfaces are discretised in
smaller areas, each area corresponding to a cell face, in such a way that boundary
data, which can be scalar or vectorial quantities, are assigned to the face center.
Dirichlet boundary conditions can be introduced assigning a set of constant
values to a certain variable, or, differently, Neumann boundary condition can
be imposed when requiring a constant gradient. Neumann boundary conditions
are implemented in OpenFoam through two different options: the zeroGradient
and the fixedGradient condition. The former is widely used and implies that
the gradient of a certain field φ is zero in the direction normal to the boundary
surface, it can be seen as a particular case of the latter option which sets the
gradient fixed to a certain value. The calculation strategy used for boundaries
definition is described carefully in this section referring to the first steady-state
simulation, which considers non reacting flows. For the following simulations
the modifications occurred to this base case, if present, will be specified.
The velocity field at the inlet was prescribed referring to the set of data pro-
vided by the University of Adelaide [20]. It is reasonable to maintain that, if the
computational domain is long enough, the flow will fully develop before reaching
the outlet. As a consequence of that, the velocity and the turbulence parame-
ters do not change as the flow progresses, condition met by the zeroGradient
specification which ensures that the gradient of a certain variable in the direc-
tion normal to the considered surface is zero. In this specific case the flow is
developing in the direction normal to the outlet surface which is coherent with
the zeroGradient imposition. The inlet velocity profile is constructed imposing
a zero radial component, on the other hand the axial component are determined
employing the tabulated values of Umean. However, the measurements are avail-
able only at specific locations which do not coincide with the grid nodal points.
Therefore, a linear interpolation was performed in order to determine the entire
inlet velocity distribution.
For what concerns the other boundaries of the domain, the symmetryPlane
condition is applied to the Axis boundary and, considering the numerical con-
straints, a zeroGradient condition is specified for the lateral surface, which is
indicated in Figure3.2 by the region ABDE. Similarly, OpenFoam requires to
specify the inlet and outlet values for the pressure. At the outlet the pressure
assumes the atmospheric value of 101325 Pa; on the other hand, at the inlet
boundary plane the zeroGradient condition was applied in such a way that the
boundary pressure values are extrapolated by the nearest cells in the internal
field. With respect to k and ε, the inlet field is determined employing approxi-
mate formulas [1]:
k =
1
2
U x
2
+ U y
2
+ U z
2
(3.1)
Urms = U x
2 + U y
2 + U z
2 (3.2)
18

Alternatively, it is not unusual to find estimations of k based on turbulence
intensity values, for which the following empirical correlation is available [19]:
k =
3
2
(IUmean)2
(3.3)
Substituting I with Urms/Umean it can be noticed how this method yields
values of k three times higher then the previous one. By analogy, approximate
inlet distributions for ε are found by means of empirical relationships as a func-
tion of the turbulent kinetic energy k as well as the turbulent length l . As can
been seen in the literature [1] [19] [3], the following equation is widely used to
initialize the turbulent kinetic energy dissipation rate inlet field:
ε = 0.164
k2
l
(3.4)
There are plenty of different approaches to characterize l which lead un-
avoidably to different scenarios, for this specific context the calculation strategy
adopted is shown in the appendix.
3.2 Cold flow results
In this paragraph the results of the initial study are presented. The accuracy of
the computational model, which intends to reproduce the real physical phenom-
ena, is validated considering a reduced study, within which combustion is not
yet included. In this way the accuracy of the underlying assumptions is corrob-
orated with respect to both physical aspects, for instance boundary conditions
or geometry definition, as well as numerical aspects, such as grid refinement or
computational time. The non reactive-flow simulation is performed with the
aid of the simpleFoam solver, which features were described in section 2.3.1.
Initially, the focus is on determining the velocity field, for which purpose the
Navier Stokes equations are solved including the pressure coupling. At this
stage, the density is assumed to be constant and equal to the atmospheric stan-
dard value (ρ = 1.2 kg/m3
), moreover, the interaction between pressure and
density is neglected. The results are summarised in Figure 3.6 and Figure 3.7.
The contour plot helps to provide insight about the velocity distribution on the
domain; the isolines showing the highest velocity values are located close to the
bottom left corner of the domain, where fuel is injected. On the other hand, the
last curve, depicted in red, refers to the coflow, which progresses at 1.1 m/s.
Figure 3.10 shows the radial velocity profiles at different heights; as can be seen,
jet divergence leads to smoother profiles for which the difference between fuel
and coflow velocity is less marked. The results are obtained for a converged
solution; in other words the solution satisfies (with a certain margin of error)
all the equations considered.
In the subsequent step the previous simulation is enriched with a further de-
tail, more specifically the mixture fraction is introduced as a new scalar variable.
19

Figure 3.6: Velocity contour plot
Figure 3.7: Mixture fraction spatial
distribution
In OpenFoam Z is introduced as a new variable for which a transport equation
needs to be solved. Therefore, appropriated boundary conditions are set, re-
quiring Z = 1 for r <= 2, 2 mm, namely in the region where fuel exudes from
the pipe; similarly, Z is null in the coflow region. In fact, the mixture fraction
is normalised in such a way that it ranges between 0 and 1, with the maximum
values corresponding to a pure fuel jet. Furthermore, the simpleFoam solver is
expanded to include the mixture fraction transport equation, which is placed in
the loop after the velocity and pressure equations. The aforementioned equation
is Eqn.2.8 included in the previous section. Finally, the results for the axial and
radial profiles of mixture fraction are shown in Figure 3.8 and Figure 3.9.
For what concerns the radial profiles, the abrupt change of Z occurring at
the interface between fuel and oxidizer can be noticed. As expected, mixture
fraction is close to unity values where the fuel is injected for both axial and radial
profiles. Furthermore, it can be observed the analogy between the profiles of
velocity and mixture fraction; this can be clarified considering the importance
of convection in high Reynolds number flows. In fact, in this case, the passive
scalar is distributed in the domain according to the velocity field, with diffusion
playing a less important role. Finally, the spatial distribution of mixture fraction
is depicted in Figure 3.7.
20

Figure 3.8: Mean mixture fraction axial profile
Figure 3.9: Mean mixture fraction radial profiles for
different heights
Figure 3.10: Velocity radial profiles for different heights
21

3.3 1D Manifold- Cold flow
The simulation is performed by means of a transient incompressible solver as
described in section 2.3.3. At the start of every iteration, the manifold is read
and the variables interpolated yielding a continuous distribution in the range of
interest. The information is then stored before solving the equations for velocity,
pressure and mean mixture fraction. In this way for these three quantities the
distribution throughout the domain is made available and the other variables
which are included in the manifold can be updated being linked to the mixture
fraction from the interpolation procedure.
Moreover, this study again refers to non reacting flows, in fact the thermo-
physical parameters such as density and viscosity are interpolated as a function
of mixture fraction considering only the points of the manifold for which holds
Y = 0; thus, since the progress variable is proportional to the mass fractions of
the chemical species produced in the combustion process, no chemical reactions
is introduced. Following this approach the look-up procedure can be tested
before loading the computational model with further details. In fact, being a
simple mixing problem it is possible to predict the patterns of representative
variables such as density and viscosity; if the results are in line with the predic-
tion the calculation strategy is validated. For instance, concerning the density,
the atmospheric value (1.2 kg/m3
) is expected on the coflow side as well as the
fuel characteristic value (0.73 kg/m3
) is presupposed along the turbulent jet,
intermediate values must occur in the rest of the domain. The same behaviour
is expected for the viscosity. As can been in Figure 2.6 and Figure 2.7, the
results corroborate the prediction offering a positive feedback for the considered
methodology.
In respect to velocity and mixture fraction patterns it can be noticed in Fig-
ure 3.11. and Figure 3.12. how they resembles the results obtained in section
3.2. The introduction of a variable density through the manifold does not influ-
ence the pressure and density estimation. In fact, pressure density interactions
are neglected, conversely, the velocity is affected by the density fluctuations in-
troduced by the manifold. However, the density of the air in the coflow, which
spreads widely the domain, has the same value used in the previous simulation.
Therefore, it is expected that, compared with the previous case, the reduction
of density brought by the fuel jet hardly affects the velocity profiles. This will
be no longer true when combustion is included resulting in a mixture massive
density drop which in turn enhance the flow expansion. Being the flow patterns
conserved, it follows that the mixture fraction, as a passive scalar quantity
transported by the flow, shows an unaltered spatial distribution. Eventually,
minor changes with respect to the mixture fraction calculation in section 3.2
could be noticed due to the different estimation of the diffusivity coefficients: in
fact, in the steady simulation the laminar diffusivity was set equal to a certain
value (the same for fuel and oxidiser) whereas in this case it is extracted from
the manifold and depends on the mixing. This in turn influences the mixture
fraction propagation acting on the diffusivity term of the transport equation;
however, it should not be forgotten that the laminar diffusion plays a less im-
22

Figure 3.11: Density spatial distribution Figure 3.12: Viscosity spatial distribution
portant role when flow velocity is high, as in the fuel jet case. To conclude,
the look-up procedure has been tested analysing the interactions between mix-
ture fraction and density; in the following section combustion is included in the
simulation by means of a 2D manifold.
3.4 2D Manifold
At this stage the progress variable is included in the look up procedure leading
to a two-dimensional interpolation for the thermophysical parameters present
in the manifold. The manifold grid is constituted by 300 points for the mixture
fraction as well as many points for the progress variable. The findings of this
simulation are shown in two different steps: firstly, the combustion process is
detected and analysed observing the results for source term, progress variable
and mixture fraction. Secondly, the focus will be on the temperature distribu-
tion for which a comparison with the experimental data is finally offered. The
results of this simulation are not obtained for a converged solution; in fact, dur-
ing run time the model withstands a progressive pressure build up that forces
the calculation to stop after a simulation time of 0.0301 s. To avoid this pres-
sure non-physical behavior different countermeasures have been tested without
remarkable improvements: these include increasing of the relaxation factors,
decreasing of the Courant number by means of smaller time steps definition,
introduction of various discretisation schemes, enhancing of the grid refinement
as well as implementation of different boundary conditions. A possible cause for
this limitation could be hidden in the pressure calculation. It is possible to see
23

Figure 3.13: Velocity radial profiles at
different heights
Figure 3.14: Mean mixture fraction radial
profiles at different heights
how to estimate the pressure the solver includes also the compressibility effect,
namely the pressure variation due to density changes. This effect is of impor-
tance at high Mach number, however, it is not usually included in commercial
CFD incompressible solvers for which pressure and density are calculated sep-
arately. Furthermore, incompressible solvers do not solve any equation for the
density which is derived from the other quantities, for instance by means of the
ideal gas law or, in the FGM method, it can be retrieved from the manifold.
However, due to the following reasoning it was judged interesting to consider
the instantaneous results for the time step t = 0.0277 s. In fact, considering
the fuel jet peak speed of 70 m/s, a residential time of 0.0028 s is found. This
value overestimates the real residential time considering how the particles, once
injected, slow down due to mixing; however, for the sake of simplicity, it is al-
lowed to estimate the calculation time of t = 0.0277 as roughly equal to ten
residential times. Moreover, with respect to thermochemical parameters such
as temperature or source term the spatial distribution distribution do not ap-
pear to fluctuate within the domain during the previous two residential times.
As the simulation progresses further there would still be variations in the solu-
tion, however, they would affect the flow further upstream, in a region which is
not captured by the considered domain. Due to this considerations the instanta-
neous results occurring at t = 0.0277 s are considered, although the performance
was not ideal. In fact, the good practice would involve averaging the results for
five to ten residential times where the solution appear to keep a constant trend.
On the other hand, the effects induced by the pressure accumulation are still
contained as it will be more clear analysing the temperature distribution.
24

3.4.1 Combustion inclusion
In this section the behaviour of progress variable and progress variable source
term is analysed. Lastly, the mixture fraction distribution is scrutinised offer-
ing an opportunity of comparison with the results of section 3.3. Regarding the
progress variable source term an overview of the manifold as well as the pro-
jection of the manifold in the Z-PV plane is offered in Figure 3.15a and Figure
3.15b.
(a) (b)
Figure 3.15: Source term profile along the manifold
As it is possible to see in Figure 3.15b the highest reaction rates occur for Z
ranging between 0.1 and 0.2, where the stoichiometric value of mixture fraction
is found. In accordance with the manifold it is also predicted that the source
term is maximum in the progress variable interval included between 0.6 and
0.9. In other words, regarding the source term, it can be recalled what stated in
section 2.1.1. In non premixed flame the chemical reactions occur at the flame
front and the flame progressively quenches when Z assumes extreme values,
namely when the oxidiser is too scarce or abundant.
25

Figure 3.16: Source term spatial
distribution
Figure 3.17: Progress variable spatial
distribution
As it is shown in the graphs 3.16. and 3.17, the findings confirm the predicted
behaviour for PV and the source term ω. The reaction rate is located at the
interface between fuel and oxidiser, moreover, at the same location the progress
variable approaches the unity value. It could also be noticed how the source
term peak value is considerably lower than the peak value shown in the manifold
representation of Figure 3.15b, this is expected to increase when the simulation
reaches the converged solution.
Finally, the results for mixture fraction radial profiles are plotted in Fig-
ure 3.19. Mixture fraction is a conserved variable in combustion processes [18],
therefore, it is expected to maintain the same patterns as in Figure 3.14. Con-
versely, as can be seen comparing the graphs in Figure 3.19. and Figure 3.14,
once combustion is introduced, the mixing becomes less homogeneous as it is
withstood by the high values of Z along the fuel jet. This can be understood
explaining that combustion is per se one of the actors, although not the only
one. In fact also transport phenomena play an important role; due to the higher
temperature the flow causing density drops, with convection becoming prepon-
derant mixture fraction patterns stretch resulting in higher values also upstream
in the domain. Furthermore, the higher the temperature the higher the viscosity
which means less mixing.
26

Figure 3.18: Mean mixture fraction radial profiles for
different heights
3.4.2 Analysis of temperature results
In this paragraph the main findings for the temperature are presented. As a
starting point a representation of the manifold is depicted in the graphs below:
(a) (b)
Figure 3.19: Temperature profile along the manifold
27

It can be observed how temperature and source term follow similar paths in
the PV-Z plane. From a physical point of view this is justified, since where the
chemical reactions are more intense also the temperature is enhanced; again, in
non premixed flame, the two phenomena are displayed together when mixture
fraction reaches the stoichiometric value. As can be seen in the contour plot
below, the isolines for the highest temperatures exactly outline the flame front,
in the same fashion as the source term in Figure 3.16.
Figure 3.20: Temperature contour plot Figure 3.21: Temperature distribution
Finally, in Figure 3.22 and Figure 3.23, the temperature axial and radial
profiles obtained in the computation are compared to the experimental data
collected by the University of Adelaide [20]. The axial profile appear to be
realistic and well-founded being considerably close to the experimental results.
As it possible to see, the region of the domain between the heights of 0.18 m
and 0.2 m is where the pressure waves accumulates, leading to the simulation
interruption. The temperature prediction can be further investigated including
the radial profiles. Those profiles refer to the heights where measurements are
also available.
28

Figure 3.22: Temperature axial profile
(a) z = 0.031 m (b) z = 0.062 m
(c) z = 0.092 m (d) z = 0.123 m
Figure 3.23: Temperature radial profiles at different heights
There is a significant agreement between the results of OpenFoam and the
experimental data, however, in comparison with the axial distribution, the link
29

between experimental and computational results becomes weaker as observable
in the temperature peak value and radial distribution. A possible explanation
for this result may involve the missing contribute of radiative heat losses in the
computational model. In fact, this would explain both the temperature overes-
timation as well as the enhanced radial expansion of the ﬂow. Regarding the
temperature estimation, without considering those losses, more energy is made
available for the chemical reactions which is per se a cause of temperature rise.
Furthermore, since hot gasses tend to expand, the higher temperature would
also enhance the displacement of the gas particles towards the radial direction.
To take into account the radiative heat losses a possible approach would involve
the improvement of the manifold, more speciﬁcally the introduction of enthalpy
as an additional controlling variable.
30

Chapter 4
Conclusions
The research aimed to illustrate the possibility of linking the FGM technique
with OpenFoam 2.1.1. in order to simulate the behaviour of a turbulent diffu-
sion flame. Initially, the attention was directed towards the construction of an
appropriate computational model with fitting geometry as well as boundary con-
ditions. To test the accuracy of the model a cold flow simulation was performed,
which lately was enhanced introducing the mixture fraction as additional vari-
able. Afterwards, the FGM method was tested focusing on the look-up routine;
in other words the model was initially coupled with a one-dimensional manifold.
Finally, in order to reproduce the combustion the progress variable was intro-
duced in the FGM database yielding a two-dimensional manifold. In respect to
the reactive flows simulation it was not possible to reach a converged solution,
however, the findings for an instantaneous solution have been analysed showing
strengths and limits of the numerical model. The temperature axial and radial
profiles have been compared with the experimental data, showing considerable
similarities.
The methodologies applied throughout the three months stint can fruitfully
be employed in analogue fields of research. More specifically, this work, devel-
oped within the Dreamcode project, is the initial step of a in depth following up
research developing within an internship at Rolls Royce Deutschland. The com-
bination of FGM with CFD codes has already demonstrated that combustion
phenomena can be reproduced with limited computational effort, thus, the fu-
ture directions of research aim to enrich the current methodologies with further
detailed models. With this respect the Eindhoven University of Technology and
Rolls Royce Deutschland are collaborating to combine the FGM method with
models for soot prediction.
31

Appendix
k and inlet boundary fields
The k inlet boundary field is determined through approximate formulas (3.1)
and (3.2). Thus, the turbulent kinetic energy values are determined for each cell
of the inlet plane starting from Urms values. Moreover, as can be seen in Figure
1, the values of I are included in the dataset, consequently a second calculation
of k is performed and the results are used to asses the robustness of the initial
evaluation.
Figure 1: Turbulent intensity as a function of the radial position
[20]
The values of I are given for negative values of r, meaning that, in com-
parison with the former estimation of k, they are disposed again in the radial
direction but towards the opposite sense. In other words they refer to another
set of measurements compared to the dataset used for Table 1. The turbulent
kinetic energy is related to the turbulence intensity through Eqn. (3.3). The
results obtained considering the second set of measurements are summarised in
the Table 2
As can be observed comparing Table 1 and Table 2, there is a significant
positive correlation between the turbulent kinetic energy values calculated with
the two aforementioned approaches, in particular for the inner part of the fuel
32

Table 1: Turbulent kinetic energy as a function of Urms
r(mm) Urms
m
s k m2
s2
0.68 4.1145 8.4649
1.08 4.8172 11.6028
1.48 5.2764 13.9202
1.88 5.1900 13.4680
2.28 1.5268 1.1656
2.68 0.2445 0.0299
3.08 0.1321 0.0087
3.48 0.0815 0.0033
3.88 0.0609 0.0018
4.28 0.0450 0.0010
4.68 0.0385 0.0007
5.08 0.0305 0.0004
5.48 0.0281 0.0003
5.88 0.0240 0.0002
6.28 0.0215 0.0002
6.68 0.0205 0.0002
7.08 0.0180 0.0001
7.48 0.0176 0.0001
7.88 0.0163 0.0001
8.28 0.0155 0.0001
8.68 0.0145 0.0001
Table 2: Turbulent kinetic energy as a function of Turbulent Intensity
r(mm) I Umean
m
s k m2
s2
-0.6 0.04 75 13.500
-0.9 0.06 72 23.522
-1.4 0.09 63 43.014
-1.7 0.10 48 33.191
-2.2 0.30 6 4.860
-2.5 0.12 3 0.194
-2.9 0.06 3 0.049
-3.3 0.04 2 0.010
-3.7 0.03 2 0.005
33

pipe. Finally, after performing linear interpolation, the values of k from Table
1 were used to model the turbulent kinetic energy distribution at the boundary
plane. Reagarding ε, Eqn. (3.4) was initially considered. For internal flows l
can be approximated as follows [4] [3]:
l = 0.07L (1)
where L is usually equal to the pipe diameter. OpenFoam, within the tutorial
of the Cavity Flow, calculates l as one fifth of the computational domain length,
therefore suggesting another estimation for ε in closed domains. However, it
should not be forgotten that the inlet boundary plane corresponds to the first
plane where measurements are taken, which is 2 mm above the fuel pipe exit.
Thus, the internal flow assumption is not entirely consistent with this case study;
moreover, observing that k ranges between 1 and 15 m2
/s2
and imposing D
equal to 4,4 mm one would obtain values of ε ranging between 600 and 30000
m2
/s3
, which is physically not acceptable. In fact, due to the dramatic velocity
at which the turbulence would be dissipated, a laminar flow would be obtained
whereas a turbulent flow is expected.
For these two reasons, ε was prescribed with a constant value of 1 m2
/s3
throughout the inlet boundary plane, following the approach shown in the Open-
Foam mixerVessel2D tutorial. In respect to the other boundary surfaces, the
geometric and physical constraints are applied in the same fashion as for k.
34

Bibliography
[1] OpenFoam 2.1.1. User Guide.
[2] OpenFOAM guide/The SIMPLE algorithm in OpenFOAM.
https://openfoamwiki.net/index.php/OpenFOAM_guide/The_SIMPLE_
algorithm_in_OpenFOAM. [Online; accessed 22-November-2015].
[3] Donini A. Advanced Turbulent Combustion Modelling for Gas Turbine Ap-
plication. PhD thesis, Technische Univeristeit Eindhoven, 2014.
[4] Saxena A. Guidelines for Specification of Turbulence at Inflow Bound-
aries. http://www.esi-cfd.com/esi-users/turb_parameters/. [Online;
accessed 19-November-2015].
[5] Sharma B., Launder B. Application of the energy-dissipation model of
turbulence to the calculation of flow near a spinning disc. Letters in Heat
and Mass Transfer, 1974.
[6] Somers B. The simulation of flat flames with detailed and reduced chemical
models. PhD thesis, Technische Univeristeit Eindhoven, 1994.
[7] de Goey P. Introduction to combustion. In Lecture notes of the Course on
Combustion.
[8] Jasak H. Error Analysis and Estimation for the Finite Volume Method with
Applications to Fluid Flows. PhD thesis, Imperial College, London, 1996.
[9] Jiang L. , Campbell I. Prandtl/schmidt number effect on temperature
distribution in a generic combustor. International Journal of Thermal Sci-
ences, 2009.
[10] Holman J. Heat Transfer. Mc Graw-Hill, 2002.
[11] Nagy J. Introduction to stationary turbulence modeling (RAS) - Part 1.
https://www.youtube.com/watch?v=IPExwi2Ar-g. [Online; accessed 22-
November-2015].
[12] Somers L.M.T. Reduced chemical models. In Lecture notes of the Course
on Combustion.
35

[13] Ferziger J.H., Peric M. Computational Methods For Fluid Dynamics.
Springer, 2002.
[14] Deen N.G. Lecture notes in Introduction to CFD (course 6EMA03), Tech-
nische Univerisiteit Eindhoven, 2015.
[15] Bern M., Marshall P. Handbook of Computational Geometry. Elsevier,
2000.
[16] Luppes R. The numerical simulation of turbulent jets and diffusion flames.
PhD thesis, Technische Univeristeit Eindhoven, 2000.
[17] Pope S. Turbulent Flows. Cambridge University Press, 2000.
[18] van Oijen J. Flamelet-Generated Manifolds: Development and Application
to Premixed Laminar Flames. PhD thesis, Technische Univeristeit Eind-
hoven, 2002.
[19] Versteeg H.K., Malalasekera W. An introduction to computational fluid
dynamics. The finite volume method. Longman Group, 1995.
[20] Mahmoud S.M., Nathan G.J, Medwell P.R., Dally B.B., Alwahaby Z.T.
Simultaneous planar measurements of temperature and soot volume frac-
tion in a turbulent non-premixed jet flame. Proceedings of the Combustion
Institute, 2014.
36

Internship_Report_Mazza (2)

Recommended

Recommended

More Related Content

What's hot

What's hot (16)

Similar to Internship_Report_Mazza (2)

Similar to Internship_Report_Mazza (2) (20)

Internship_Report_Mazza (2)