Jérôme Helie

Marc Massot

Gregory Pinon

Alberto Andres

Aqeel, Benjamin, Chanisa, Damien Antonio

Eliot, Erwan, Fred, Geoffroy, Jorge Leonardo

Manu, Marina, Marc Lila

Marcos Nelson

David Uystepruyst d'avoir fait le déplacement jusqu'au laboratoire CORIA et d'avoir évalué mon travail.

Grand merci à mes deux encadrants de thèse, Julien Réveillon et François-Xavier Demoulin, de m'avoir donné la possibilité de travailler sur ce sujet de thèse, de m'avoir soutenu et guidé pendant ces trois années. Si ces

Axial velocity along jet center line at two different instants, using either Weakly Compressible SPH method either an incompressible Finite Volume method. . . . 4.9

Transverse profiles of axial velocity, at x = 9D and two different instants, using either Weakly Compressible SPH method either an incompressible Finite Volume method. . . . Mesh refinement at the gas and liquid nozzle exits, along with the number of cells in radial direction at liquid nozzle exit. . . . . . . . . . . . . . . . . . . . . . . . 5. [START_REF] Safdari | Improved multiphase smoothed particle hydrodynamics[END_REF] LES performed in the coaxial atomizer configuration of Stepowski et al. [START_REF] Stepowski | Measurement of the liquid volume fraction and its statistical distribution in the near development field of a spray[END_REF]. . . . 5.4 Measured CPU gain between medium zonal RI and medium RI simulations. . . . 5.5 Estimated CPU gain between medium zonal and medium simulations in (a) and fine zonal and fine simulations in (b). . . . . . . . . . . . . . . . . . . . . . . . . 5. [START_REF] Groenen | Les représentations de mains négatives dans les grottes de gargas et de tibiran (hautes-pyrénées). approche méthodologique[END_REF] LES configurations using a combustion chamber size domain in the coaxial atomizer configuration of Stepowski et al. [START_REF] Stepowski | Measurement of the liquid volume fraction and its statistical distribution in the near development field of a spray[END_REF]. . . . . . . . . . . . . . . . . . . . . . 5.7 Measured CPU gain between large zonal and standard runs using a medium effective mesh resolution near the injector. . . . . . . . . . . . . . . . . . . . . . .

List of Tables

Chapter 1 Introduction 1.1 General context

Atomization refers to the process of breaking up bulk liquids into droplets. Droplet cloud that is obtained is called a spray. Speaking about "process" does not necessarily mean industrial process. One of the first utilization of atomization by human that occurred in history was confection of rock painting. To obtain a negative hand print, as illustrated in figure 1.1, a hand was pressed against the wall and paint was projected using a tube or directly vaporized by spitting with the mouth [START_REF] Groenen | Les représentations de mains négatives dans les grottes de gargas et de tibiran (hautes-pyrénées). approche méthodologique[END_REF]. This technique, that was good for cave painting, is still up to date since liquid-gas atomization have taken an important place in many industrial applications, including: combustion (spray combustion in furnaces, gas turbines, diesel engines and rockets), industrial process (spray drying, spray cooling and spray painting), agriculture (crop drying, pesticide spraying), medicine (aerosol therapy) and meteorology. For instance, spray cooling is used in metal industry in the thermomechanical processing of metal alloys. Water atomization is used to cool down the hot laminated plate. To ensure that the metal keeps its isotropic properties, cooling spray must be as spatially homogeneous as possible. The subject of atomization is wide ranging and important.

Most of developments and research projects about atomization concern fuel atomization field. Fuel atomization is part of the combustion process that occurs in gas turbines (aeronautic and power generation industries) and internal combustion engine (automotive industry). The processes of liquid atomization and evaporation are of fundamental importance to the performance of a combustion system. Normal liquid fuels are not sufficiently volatile to produce vapor in the amounts required for ignition unless they are atomized into a large number of droplets with increased surface area. The smaller the droplet size, the faster the rate of evaporation. The influence of drop size on ignition performance is of special importance, because a small increase of mean drop size leads to a large increase of ignition energy. Spray quality also affects stability limits, combustion efficiency and pollutant emission levels. Homogeneity of the mixing is a key point in combustion chambers. Inhomogeneous release of the fuel can leads to some richer mixing regions inside the chamber and it will directly impact combustion and pollutant generations. The ideal spray is thus a spray composed of very small and equitably spread droplets.

With more restrict-full legislations in Europe about the emission of pollutant gases, as for instance with EURO VI norm in automotive industry and ACARE [START_REF]About acare[END_REF] in aeronautic industry, car and aircraft companies aim to increase engine efficiencies and to reduce pollutant emissions.

Improving the performances brought by the atomization process comes by a better understanding of the basic atomization process and the mastering of capabilities and limitations of all the relevant atomization devices. In particular, it is important to know which type of atomizer is best suited for any given application and how the performance of any given atomizer is affected by variations in liquid properties and operating conditions.

Until recently, studies of injectors was generally realized by a series of experimental tries for different injector geometries and operating conditions.This approach has however several limitations. First limitation is the important cost that implies the manufacturing of an injector prototype for each geometry. Second limitation is related to the difficulty to set up accurate and non intrusive measurement methods for complex geometries and realistic operating conditions.

In the face of these limits, and with the development of supercalculator capacities, car and aircraft manufacturers use more and more numerical simulation tools that offer a complementary approach with reduced costs.

Despite significant progress during the past decade, modeling and simulation of the atomization process remains a challenging problem from both the physical and the numerical point of views because of its multiscale and multiphysic character: droplets are the size of a micrometer, the nozzle orifice diameter is a few fraction of millimeters and the combustion chamber of dozen of centimeters. Atomization is also a multiphysic process, involving fragmentation of the liquid core into a droplet cloud (multiphase flow) that will vaporize (heat transfer) and ignite if spray is sufficiently homogeneous (combustion). It is thus necessary to develop new numerical methods that deal with these multiscale and multiphysic aspects to be able to simulate atomization process, with both reasonable costs and accurate predictions. In red: processes that have been modeled wit the numerical solver developed in this thesis. In orange: processes that can be potentially modeled in perspective.

Atomization of a liquid jet 1.2.1 Principal types of injectors

The purpose of an injector is to introduce the liquid fuel into a combustion chamber and, at the same time, to favor the mixing of the combustive agent and the combustible, in order to optimize the conditions of combustion. In industry, at least three main configurations of injector can be distinguished [START_REF] Arthur | Atomization and sprays[END_REF][START_REF] Clayton T Crowe | Multiphase flow handbook[END_REF]:

• Pressure atomizers or single fluid atomizers: In these devices, high pressure forces the liquid to flow at high velocity through a small opening into a steady ambient atmosphere. Velocity difference between liquid and gas leads to the disintegration of liquid until obtaining a droplet clouds. This type of injectors are widely used in industries, such as agriculture, cosmetics, automotive motors or aeronautic motors. They have the benefit to be simple and cheap to manufacture. Droplet sizes can be controlled by adjusting the injection pressure: the higher the pressure, the smaller the droplets. On the other hand, the necessary energy to atomize the fluid increases very rapidly with the mass flow rate.

• Airblast atomizers or twin fluid atomizers: These devices exploit the shear effect of an accelerated air flow parallel to the fuel. In principle, these mechanisms work at low relative speed and high air flow, as it happens for aircraft engines. Small part of high pressure air leaving out compressor stages is substituted and used in these injectors. Airblast atomizers have the benefit that, for a given mass flow rate, less energy is necessary to atomize the liquid, in comparison with a pressure atomizers. Higher fuel flow rate can thus be obtained. It is nevertheless necessary to have a high velocity gas flow to obtain a satisfying mixing.

• Rotary atomizers: Liquid is introduced at the center of a high-speed rotating disk. It is submitted to centrifugal forces and flows radially outward across the disk. At high flow rates, ligaments or sheets are generated at the edge of the disk and disintegrate into droplets. In contrast to pressure nozzles, rotary atomizers allows independent variation of flow rate and disk speed, thereby providing more flexibility in operation.

Atomization process

Atomization process is the mechanism that leads to increase the liquid-gas interfacial area inside a given control volume. Inside combustion chambers, this process is a crucial point. The different steps leading to combustion inside a combustion chamber can be summed up by the scheme in figure 1.2. The starting point is the fuel atomization. Atomization process leads to pulverization of the liquid jet into multiple droplets which, under influence of atomization mechanisms, become smaller and smaller. Evaporation of the spray release fuel vapors inside the chamber that, if it is sufficiently well mixed, will be ignited and lead to the combustion process. These four steps (atomization, evaporation, mixing and combustion) need to be mastered to obtain an ideal compromise between pollutant emissions and combustion efficiency.

These phenomena are usually studied separately, because a complete study of the whole process is hardly achievable and very complex. It illustrates well the multiphysic aspect of the combustion process happening inside a combustion chamber. A numerical method has been developed during this thesis and applied to the two first steps of the global atomization process: atomization itself and dispersed spray. These steps are highlighted in red in figure 1.2. The perspectives of this numerical method is to include also evaporation (highlighted in orange).

Two phase flow regimes 23

Atomization process can be split in three distinctive zones: primary atomization, secondary atomization and dispersed spray (see figure 1.3). These zones show particular properties that we propose to describe in next two sub-sections.

Primary Atomization or Dense zone

Primary atomization process occurs once liquid has left the injector nozzle. In this region, the high velocity gradients between the liquid and the gas lead to shearing instabilities. These instabilities show sinusoidal waves at the liquid-gas interface in the direction of the liquid flow.

The waves amplitude will increase until provoking detachments of liquid structures from the liquid core. These structures remain relatively big compared to the liquid core size. This region where instabilities and first liquid detachments appear is called primary atomization zone, also dense zone of the spray.

Secondary atomization and diluted zone

Secondary atomization follows the primary atomization. Liquid structures leaving the primary atomization area may interact between them. Two typical interactions are coalescence and collision. In the coalescence case, two liquid structures encounter each other and unified to form a single entity. In the collision case, the two structures have different velocities and encounter each other in a more violent way that provoke their breakup and the creation of smaller structures [START_REF] Jiang | An experimental investigation on the collision behaviour of hydrocarbon droplets[END_REF][START_REF] Qian | Regimes of coalescence and separation in droplet collision[END_REF].

Further from injector, liquid structures do not interact each other any more (or very weakly). At this scale, surface tension prevails. It minimizes the droplet surface and energy, leading to spherical droplets. This zone is called diluted or dispersed spray region.

Two phase flow regimes

The complex nature of two-phase flow, characterized by turbulence, deformable phase interface, phase slip and compressibility of the gas phase, makes it difficult to obtain reliable models. First of all, the nature of the flow needs to be characterized. A two-phase flow could be classified according to the state of different phases or components (gas/solids, liquid/solids, gas/particle or bubbly flows and so on). In the context of atomization and this work, only one type of two-phase flow is considered: a liquid phase and a gas phase separated by a well defined liquidgas interface. Liquid-gas flows can be broadly classified into three categories: separated flows, mixed flows and dispersed flows [START_REF] Ishii | Thermo-fluid dynamics of two-phase flow[END_REF][START_REF] Rusche | Computational fluid dynamics of dispersed two-phase flows at high phase fractions[END_REF]. Generally, each one of these categories necessitate dedicated approaches for their description.

• In separated flows, each phase is continuous and occupies a distinct region of the domain; volume fraction of primary phase is high in a region and low in the other one and both phases are separated by an interface, where surface tension force applies. Dense flow description is particularly adapted for the primary atomization region, where the liquid jet and the gas phase are still well separated.

• In dispersed flows, one phase is assumed to be dilute, with a volume fraction smaller than 10% the global volume, and composed of finite spherical inclusions dispersed inside the other carrier phase. All dispersed elements are assumed to be very small compared to the scale of the system. Dispersed flow description is particularly adapted for the dilute spray region, where liquid structures show low volume fraction and are independent of each other.

• Mixed flows are transitional states between the two other flow regimes previously mentioned. Typically, secondary atomization zone is a mixed flow region. The atomization process as a whole is considered as well as a mixed flow.

Two phase flow numerical methods

Any numerical methodology consists of a model and a solution procedure. A model is a mathematical representation of the physical process to be predicted or simulated. Models usually neglect some less important or less influential phenomena [START_REF] Rusche | Computational fluid dynamics of dispersed two-phase flows at high phase fractions[END_REF].

The dynamics of many two-phase flows encountered in engineering application are adequately modeled by the Navier-Stokes equations, that include momentum and continuity equations, a Newtonian law of viscosity and an equation of state -heat and mass transfer as well as chemical reactions and phase changed are not considered.

Three approaches are generally encountered in literature for treating two-phase flows: Euler-Lagrange model, two-fluid model and single-fluid model. Less common, meshless particle methods are also good candidates for treating interfacial flows. An overview of these four approaches is given in the next subsections.

Euler-Lagrange or Dispersed phase model

The dispersed phase model assumes that the topology of the two-phase flow is dispersed. The two phases are therefore referred to as the continuous and the dispersed phase. A macroscopic description of the dispersed phase is obtained by replacing the microscopic conservation equations with a discrete formulation. In this discrete formulation, the dispersed phase is represented by individual particles, which are tracked through the flow domain by solving an appropriate equation of motion. The equation of motion is the conservation equation of momentum expressed in the Lagrangian formulation, in which the dependent variables are the properties of material particles that are followed in their motion. Concerning the continuous phase, the conservation equations are expressed in the Eulerian frame, where the fluid properties are considered as functions of space and time in an absolute frame of reference. Navier-Stokes equations constitute the conservation equations of the continuous phase. Because of this mixed treatment of the two phases, the dispersed phase model is also referred to as the Euler-Lagrange model [START_REF] Rusche | Computational fluid dynamics of dispersed two-phase flows at high phase fractions[END_REF].

For sufficiently dilute suspensions, where the particle size is small, the influence of the dispersed phase on the motion of the continuous phase can be neglected. The coupling between the phases is then said to be one-way. However, the matter is somewhat complicated if the motions of the continuous and the dispersed phase are closely coupled, i.e. the continuous phase influences the motions of the particles and vice versa. This two-way coupling can be taken into account in the dispersed phase model with relative ease and is done by accounting for the influence of the disperse phase in the momentum equation with an extra source term [START_REF] Clayton T Crowe | Multiphase flows with droplets and particles[END_REF].

In figure 1.4-(a), Euler-Lagrange model is illustrated. The velocity of continuous phase, fluid 1, and dispersed phase, fluid 2, are respectively red and blue arrows. The continuous phase, described in an Eulerian manner, is discretized in a computational fixed mesh and velocities vector are located at the cell centers. The dispersed phase, described in a Lagrangian way, is discretized with individual particles, colored in cyan.

An Euler-Euler method: Two-fluid model

In the two-fluid model, both phases are described using Eulerian conservation equations. Each phase is treated as continuum, with its own set of governing balance equations, and owns a velocity and a pressure field. Phase fraction α is introduced into governing equations, which is defined as the probability that a certain phase is present at a certain point in space and time [START_REF] Paul | The computer simulation of dispersed two-phase flow[END_REF]. Equations are also averaged in order to preserve mass and momentum conservation of the overall flow.

In figure 1.4-(b), Two-fluid model is illustrated. The velocity of each phase is represented by one set of velocity vectors, which are shown in red and blue for fluid 1 and 2, respectively. The phase fraction of the dispersed phase is shown by small numbers in the lower right corners of the cells.

Due to the loss of information associated with the averaging process, additional terms appear in the averaged momentum equation for each phase, which require closure. An extra term that account for the transfer of momentum between the phases appears. This term is known as the averaged inter-phase momentum transfer term and accounts for the average effect of the forces acting at the interface between continuous phase and the particles, or between the two continuous phases, depending on the topology of the flow. To sum up, the two-fluid model incorporates two-way coupling.

The two-fluid methodology is applicable to all flow regimes, including separated, dispersed and mixed regimes, since the topology of the flow is not prescribed.

Single-fluid model

In single-fluid models, only one set of governing equations is used for the whole two-phase flow. Therefore, the two-phase flow can be regarded as a single-fluid flow, with a single velocity and a single pressure, composed of two species. Distinction between carrier and discrete phases is avoided and the topology of the interface between the two phases is determined as part of the solution. Let us describe four types of single-fluid models there after.

Volume of Fluid method

Volume Of Fluid (VOF) method is an interface capturing method that gives an implicit representation of the interface. This method is one of the first interface capturing method to have been developed. It has been proposed by Hirt and Nichols in 1981 [START_REF] Hirt | Volume of fluid (vof) method for the dynamics of free boundaries[END_REF] and it is based on mass conversation principle. Initially, volume fraction of liquid (or gas) is distributed over the whole computational domain, then transported by the velocity field. To better understand definition of volume fraction, we quote the original paper [START_REF] Hirt | Volume of fluid (vof) method for the dynamics of free boundaries[END_REF], adapted to our notation:

"Suppose [...] that we define a function α whose value is unity at any point occupied by fluid and zero otherwise. The average value of α in a cell would then represent the fractional volume of the cell occupied by fluid. In particular, a unit value of α would correspond to cell full of fluid, while a zero value would indicate that the cell contained no fluid. Cell with α values between zero and one must then contain a free surface."

In other words, the volume fraction α allows to access following informations in each cell:

     α = 1
⇐⇒ liquid phase , α = 0 ⇐⇒ gas phase , 0 < α < 1 ⇐⇒ contains interface .

(1. 1) In figure 1.4-(c), VOF method is illustrated. The velocity of the single-fluid mixture is represented by purple velocity vector. The phase fraction of fluid 2 is shown by small numbers in the lower right corners of the cells.

VOF methods are robust regarding topological changes since they are implicit. Volume conservation is guaranteed by transporting volume fraction but if mesh is not fine enough, parasite effects may occur in singular zones as disintegration of a filament in spherical spots. This phenomenon, called numerical surface tension [START_REF] Db Kothe | Volume tracking of interfaces having surface tension in two and three dimensions[END_REF], seems unavoidable with Eulerian formalism when interface structure width is of the same order than cell size. VOF methods are thus poorly adapted for dispersed flows unless the mesh is fine enough, but it can lead to prohibitive computational costs.

One of the main drawback in VOF method is the difficulty to compute geometric characteristics of the interface (normal n and curvature κ) that allows to calculate the surface tension. As shown with equation (3.3), α transport equation provides informations for locating the interface but not for defining its geometric characteristics explicitly. It is thus necessary to use interface reconstruction methods.

One of the first interface reconstruction method to be proposed is the SLIC (Simple and Line Interface Calculation) method, in 1976 by Noh and Woodward [START_REF] William | Slic (simple line interface calculation)[END_REF]. In this method, considering a Cartesian mesh, interface is approximated in each cell, as segments (or planes in three dimensions), aligned with one of the mesh coordinates. This direction depends on flow direction.

The PLIC (Piecewise Linear Interface Calculation) [START_REF] Douglas | Comments on modeling interfacial flows with volume-of-fluid methods[END_REF] is more accurate than the SLIC method. In PLIC, an interface within a cell is approximated by a segment with a slope determined from the interface normal. The resulting fluid polygon is then used to compute fluxes through any cell face.

An alternative to geometric reconstruction algorithms is to avoid interface reconstruction by using an interface compression method. Its principle lies on correcting the numerical diffusion of liquid volume fraction α in the advection equation with a compression term. This compressive scheme benefits from a high resolution differencing schemes to calculate volume fluxes [START_REF] Ubbink | Numerical prediction of two fluid systems with sharp interfaces[END_REF]. Additionally, the implementation of compressive algorithms on arbitrary unstructured meshes is quite straightforward. This method is used in OpenFOAM R VOF solver [START_REF] Weller | Derivation, modelling and solution of the conditionally averaged two-phase flow equations[END_REF][START_REF] Weller | A new approach to vof-based interface capturing methods for incompressible and compressible flow[END_REF], namely interFoam. Equations of this treatment will be more detailed in section 2 of chapter 3.

VOF method has been recently used for simulation of primary atomization in airblast atomizer by Tian et al. [START_REF] Xiu-Shan Tian | Threedimensional large eddy simulation of round liquid jet primary breakup in coaxial gas flow using the vof method[END_REF] and in a high-pressure diesel atomizer by Ghiji et al. [START_REF] Ghiji | Cfd modelling of primary atomisation of diesel spray[END_REF]. One can cite also the team of Zaleski, that principally uses VOF method [START_REF] Fuster | Simulation of primary atomization with an octree adaptive mesh refinement and vof method[END_REF][START_REF] Tomar | Multiscale simulations of primary atomization[END_REF].

Level Set

Level Set method was initially proposed by Osher et al. in 1988 [27]. In this method, a passive scalar that represent the interface is transported. This scalar value is basically equal to the signed distance from the considered mesh cell to the interface. Therefore, the surface is defined as the one on which the level-set function ϕ = 0. This property must be fulfilled during the simulation and a technique of re-initialization ensures it [START_REF] Sussman | A level set approach for computing solutions to incompressible two-phase flow[END_REF].

As in VOF methods, fluid properties are determined by the local value of ϕ. Only the sign of CHAPTER 1. INTRODUCTION ϕ matters. The variable ϕ allows to access following informations in each point of the field:

     ϕ > 0 ⇐⇒ liquid phase , ϕ < 0 ⇐⇒ gas phase , ϕ = 0 ⇐⇒ interface . (1.2)
The advantage of this approach relative to the VOF scheme is that ϕ varies smoothly across the interface while the volume fraction α is discontinuous there. This method is one of the simplest to describe and capture interface, it allows also to obtain geometric characteristics of the interface, as normal n and curvature κ, in a simple and accurate way (second order accurate).

However, the original level-set method does not exactly conserve mass, particularly in high shear flow or for coarse meshes. Several improved methods have been proposed to mitigate this conservation problem.

One can cite the Accurate Conservative Level Set (ACLS) proposed by Osson and Kreiss [START_REF] Olsson | A conservative level set method for two phase flow[END_REF]. Similarly to the interface compression method developed by Weller in VOF [START_REF] Weller | Derivation, modelling and solution of the conditionally averaged two-phase flow equations[END_REF], this ACLS method is based on the implementation of an interface compressive term in the transport equation of ϕ. This concept was used by Desjardins for the simulation of diesel jets [START_REF] Desjardins | An accurate conservative level set/ghost fluid method for simulating turbulent atomization[END_REF].

One can cite also the coupled VOF-LS method (CLSVOF), that use the mass conservative description of VOF to alleviate this issue from LS. It has been proposed Sussman and Puckett [START_REF] Sussman | A coupled level set and volume-of-fluid method for computing 3d and axisymmetric incompressible two-phase flows[END_REF]. It consists to compute each method independently at the beginning of the time-step then to couple them. In each cell containing the interface, the interface described by LS is slightly displaced following interface normal so that the liquid volume computed with LS corresponds exactly to the volume calculated with VOF. Geometric characteristics of the interface are still extracted from Level Set that provides a better accuracy. The main drawback is the computational cost of such method. It has been used for simulating diesel jets by Menard et al. [START_REF] Ménard | Coupling level set/vof/ghost fluid methods: Validation and application to 3d simulation of the primary break-up of a liquid jet[END_REF], Desjardins et al. [START_REF] Desjardins | Direct numerical and large-eddy simulation of primary atomization in complex geometries[END_REF] and airblast atomization by Xiao et al. [START_REF] Xiao | Les of turbulent liquid jet primary breakup in turbulent coaxial air flow[END_REF] for instance.

Diffuse Interface models

Diffuse interface models are single-fluid, as VOF and LS, with the difference that the interface is not tracked and computed anymore but described as a diffuse interface. We shall describe more precisely one of this model, i.e. the ELSA model (Euler Lagrangian model for Spray Atomization) that aims to model the different stages of atomization. This method was initially proposed by Vallet and Borghi in 1999 [START_REF] Vallet | Modélisation eulerienne de l'atomisation d'un jet liquide[END_REF]. It introduces the interface area density, which indicates the quantity of interfacial aera in each cell, but without indications of the shape of the structures. In that way, the interface density can treat as well a spherical droplet in the dispersed spray region as the distorted liquid core in the primary atomization region. This model is based on the assumption that turbulence is the main mechanism leading to detachment of liquid structures in the secondary atomization region. It is at the opposite of other models, as the WAVE model [START_REF] Reitz | Modeling atomization processes in high-pressure vaporizing sprays[END_REF], that consider Kelvin-Helmotz instabilities [START_REF] Deneys | Atomization and other breakup regimes of a liquid jet[END_REF] the fundamental mechanism leading to detachments, not turbulence. It can necessitate adaptations of ELSA model depending on injector type and geometry. Lebas [START_REF] Lebas | Modélisation Eulérienne de l'Atomisation Haute Pression-Influences sur la Vaporisation et la Combustion Induite[END_REF] shows that the turbulent aspect 1.5 Two phase flow and turbulence 29 seems sufficient when this model is applied on pressure atomizer configurations. However, for instance, Demoulin et al. [START_REF] Demoulin | A new model for turbulent flows with large density fluctuations: Application to liquid atomization[END_REF] show that, for airblast atomizers, ELSA model needs to be adapted by considering Rayleigh-Taylor instabilities to obtain good agreement between simulation and experience regarding mean liquid penetration. In the last chapter of this document, large eddy simulations with ELSA model are applied on the same airblast atomizer configuration [START_REF] Stepowski | Measurement of the liquid volume fraction and its statistical distribution in the near development field of a spray[END_REF], and same observation is drawn: The mean liquid penetration in primary atomization region is not correctly captured. This difference may be linked to a similar comparison discussed in the thesis of P.A. Beau [START_REF] Beau | Modélisation de l'atomisation d'un jet liquide-Application aux sprays Diesel[END_REF]: The single-phase approach of the turbulent model, here LES, is the cause of the prediction deficiency. An evolution of the turbulent model from a single-phase to a two-phase approach should be considered.

Meshless particle methods

Using meshless particle methods is a popular approach circumventing the mesh tangling problem. The flow is discretized with a finite number of particles which carry the fluid characteristic properties such as position, mass, velocity, and other hydrodynamics properties. Then, the fluid system evolution is governed by interactions between these particles. In the framework of meshless particle methods, Smoothed Particle Hydrodynamics (SPH) is a solution towards achieving a realistic physical model for interfacial flows. Based on a smoothing kernel function, physical quantities are interpolated in a discrete form [START_REF] Leon | A numerical approach to the testing of the fission hypothesis[END_REF][START_REF] Robert | Smoothed particle hydrodynamics: theory and application to non-spherical stars[END_REF]. The main advantages of the SPH approach for treating two phase flows are the following: (i) natural distinction between phases due to holding material properties at each individual particle and (ii) non-existence of convective term in discretization of the momentum equation, due to the Lagrangian formalism. This latter point allows to avoid the numerical diffusion that occurs in Eulerian formalism when a scalar is transported by the flow. Nevertheless, efforts for developing and applying the SPH method in the field of fluid dynamics have been less important in comparison with the finite volume method. The standard SPH method in its current stage has some shortcomings: (i) modeling of large ratios of density/viscosity discontinuity at the interface, and (ii) particle clustering in some region that may cause insufficient particle resolution in some other region [START_REF] Safdari | Improved multiphase smoothed particle hydrodynamics[END_REF].

Hoefler et al. [START_REF] Hoefler | Multiphase flow simulations using the meshfree smoothed particle hydrodynamics method[END_REF] have treated primary atomization with SPH in airblast configuration. This is the most advanced SPH simulation of primary atomization in our knowledge.

In figure 1.4-(d), SPH method is illustrated. The whole mixture is discretized in a Lagrangian formalism and described by the displacement of each particles. The fluids and 1 and 2 are respectively marked by white and blue particles, which are convected by their own velocity, represented with purple arrows.

Two phase flow and turbulence

Turbulence flow regimes, in contrast with laminar flow regimes, are characterized by velocity and pressure fluctuations and the presence of eddies with many different scales. Turbulence is maintained through a energy transfer process, namely energy cascade, that occurs from the most energetic eddies to the smallest ones. Energy is dissipated through viscosity effects when reaching the smallest eddy scales. This process is known as the theory of energy cascade of

CHAPTER 1. INTRODUCTION

Kolmogorov [START_REF] Nikolaevich | The local structure of turbulence in incompressible viscous fluid for very large reynolds numbers[END_REF]. The higher the Reynolds number, the greater the range of scales.

Turbulence thus contains a broad range of scales. To run a Direct Numerical Simulation (DNS), all these scales must be taken into account, in particular the Kolmogorov scale, i.e. the smallest scale of the flow, that dissipates energy. The size of the discretization elements of the computational domain is close to the Kolmogorov scale. Thus, for large Reynolds number flows, it leads to a very large number of elements and, as a consequence, a prohibitive computational cost. Considering current computer performances, DNS are limited to academic studies of low Reynolds number flows and it is far for being used in industrial applications. Therefore, when one considers high Reynolds number flows, turbulence modeling approaches must be considered.

The cheapest turbulence approach, computationally speaking, is the Reynolds Averaged Navier-Stokes (RANS) that consists in averaging the flow properties. Navier-Stokes equations are averaged and additional unknowns appear as the unclosed Reynolds stresses. To close the system of equations, additional transport equations are solved, from zero for mixing length model, to seven for Reynolds stresses model. One of the most known model is the k -ε model, that solves two additional transport equations. RANS model are generally preferred in industry.

Large Eddy Simulation (LES) approach is the second family of turbulent models and consists to model only the smallest scales of the flow, in which viscous dissipation becomes preponderant. The large scales are simulated without any modeling. Compared to RANS, LES induces an increase of computationall resources but it allows to access to some specifies, such as large scale unsteady effects [START_REF] Stephen B Pope | Turbulent flows[END_REF][START_REF] Lesieur | Turbulence in fluids[END_REF].

If one performs numerical simulation of primary atomization, one shall apply one of the three approaches described previously, i.e. DNS, RANS or LES. As in turbulent flow of a single-phase fluid, multiphase flows possess a large range of scales, ranging from the size of a smallest dispersed phase structure to the size of the system under investigation. In primary atomization process, thickness of ligaments and droplets that follows the break-up of the interface can be smaller than the Kolmogorov length scale. DNS of such flows without any modeling of the two phases aspect is thus not affordable. Two-fluid models may be used for DNS of two-phase flows, showing low Reynolds number. Boeck et al. [START_REF] Boeck | Ligament formation in sheared liquid-gas layers[END_REF] used VOF for full numerical simulations of two-phase liquid-gas sheared layers, with the objective of studying atomization. One of the first DNS of primary atomization was performed by Menard et al. [START_REF] Ménard | Coupling level set/vof/ghost fluid methods: Validation and application to 3d simulation of the primary break-up of a liquid jet[END_REF], with a LES methodology coupled with VOF (CLSVOF), to study the primary break-up process. In this work, injection speed was deliberately reduced, in order to increase the size of the smallest droplets in the secondary atomization region, hence to reduce the mesh size and the computational costs. Desjardins et al. [START_REF] Desjardins | An accurate conservative level set/ghost fluid method for simulating turbulent atomization[END_REF] run a DNS/ACLS of a turbulent atomization of liquid diesel jet. Shinjo and Umemura [START_REF] Shinjo | Simulation of liquid jet primary breakup: dynamics of ligament and droplet formation[END_REF] studied also primary atomization in a pressure atomizer using DNS/CLSVOF. Purpose of these previous works are to study physical phenomena in primary atomization and to serve as reference for validating other modeling approaches, as RANS and LES models. Nevertheless, they involve a quite small area, limited by a few injector diameters in the downstream direction. Simulating the whole atomization process going until several hundred of diameters in the downstream direction is hardly feasible with DNS.

Since [START_REF] John K Dukowicz | A particle-fluid numerical model for liquid sprays[END_REF], the industrial approach uses RANS system with Euler-Lagrange models: Eulerian for the gas phase associated with a Lagrangian solver "reproducing" the presence of physical particles inside the domain. Based on a wrong hypothesis considering models for non-dense flow at the injection, correct results can be obtained thanks to the convective characteristics of the Lagrangian method. Despite the fact that the provided results are rough, this approach has been widely adopted because of its ability to model the whole spray, from the nozzle outlet to the mixing area inside the combustion chamber, even if the flow is inaccurate at the nozzle outlet. RANS can be combined also with single-fluid models, as ELSA and two-fluid models [START_REF] Eric | Atomization modeling of liquid jets using an Eulerian-Eulerian model and a Surface Density Approach[END_REF].

Application of LES formalism to solve primary atomization is relatively recent. LES are an intermediate tool between DNS and RANS, by mitigating the fine mesh constraint. One classical approach consists to combine the single-phase turbulent LES model with an interface capturing method as VOF or LS. Good results have been obtained when applying LES/VOF on primary atomization [START_REF] Srinivasan | Numerical investigation on the disintegration of round turbulent liquid jets using les/vof techniques[END_REF][START_REF] Xiu-Shan Tian | Threedimensional large eddy simulation of round liquid jet primary breakup in coaxial gas flow using the vof method[END_REF]. Recent developments tend to take in account the issue of liquid structures that are smaller than the mesh size. Subdgrid methods for smallest spray droplets have been developed and applied for simulating primary atomization in Diesel jets [START_REF] Herrmann | A parallel eulerian interface tracking/lagrangian point particle multiscale coupling procedure[END_REF][START_REF] Chesnel | Subgrid analysis of liquid jet atomization[END_REF] and airblast atomizer configurations [START_REF] Xiao | Large eddy simulation of liquid jet primary breakup[END_REF][START_REF] Xiao | Les of turbulent liquid jet primary breakup in turbulent coaxial air flow[END_REF]. LES has a great potential for modeling accurately atomization process however computational costs are still too high to be able to treat both primary atomization region and mixing, evaporation and combustion zones.

Objectives

Despite significant progress during the past decade, modeling and simulation of atomization process, with mixed flow regimes and a wide range of characteristic scales, remains a challenging problem from both the physical and the numerical point of views. Accordingly, several authors combined multi-scale resolutions in different ways. The simplest one is to properly refine the mesh close to the injector nozzle and then to have a lower mesh resolution further downstream, therefore, allowing a complete combustion zone. Nevertheless, for atomized liquid jets, despite enlargement of the length scale of the dynamic field, the scale of the spray decreases or at least remains very small. This scale separation between dynamic and liquid field requires either (i) to keep a very fine mesh at the liquid gas interface even far away from the injector -this can be done locally and dynamically modified via Adaptive Mesh Refinement approaches (more details about these approaches will be given in chapter 3) -or (ii) to physically change the approach to represent the spray. This work focus on the point (ii).

Therefore, the objective of this work is to address this multi-scale issue of the atomization process by developing an hybrid numerical method, or more precisely, a multi-approach and multi-scale methodology, that divides the flowfield into two zones: a inner zone dedicated to solve the primary and secondary atomization regions and a outer zone for the rest of the field.

This hybrid method will have to satisfy the following criteria:

• It must couple two different domains in which different numerical methods are used to solve the flow. Hence the multi-approach aspect of the method.

• Each domain must be as independent as possible, i.e. with their own discretization schemes and physical models. One domain will be refined in time and space compared to CHAPTER 1. INTRODUCTION the other.

• The inner zone is a small-size fine scale local problem which is solved separately and whose solution is used to construct an approximate global fine-scale solution in the underlying outer zone. Hence the multi-scale aspect of the method [START_REF] Hajibeygi | Multiscale finite-volume method for parabolic problems arising from compressible multiphase flow in porous media[END_REF].

• It must be as accurate and conservative as possible.

As mentioned before, the idea of this solver is to keep a strong resolution in the primary atomization where the strongest velocity and volume fraction gradients have to be resolved but to allow a coarser mesh size further in the dispersed spray region. To correctly capture the dispersed phase flow in the diffusive regions, the single-fluid ELSA model will be used. By treating the interface as a surface density variable in each cell, it allows to use a low mesh resolution in these regions and hence to decrease computational costs. It can as well capture the separated flow in the primary atomization region but here the low resolution of the global domain will have an impact on the solution. Hence a correction of the global solution by a local domain is necessary.

In the inner zone, an appropriate approach will be used to correctly capture the interface destabilization and liquid structures detachment, such as the Volume Of Fluids (VOF) method. VOF method is conservative, robust and capable of treating small-case interface topologies such as breakup and reconnection. It has been successfully applied for simulating primary atomization, using LES for instance [START_REF] Xiu-Shan Tian | Threedimensional large eddy simulation of round liquid jet primary breakup in coaxial gas flow using the vof method[END_REF][START_REF] Ghiji | Cfd modelling of primary atomisation of diesel spray[END_REF]. Associated with a compressive scheme for the interface reconstruction, VOF is therefore a good candidate for solving the primary and secondary atomization regimes. Furthermore, it is a single-fluid model, that can be easily coupled with the ELSA model.

Smoothed Particle Hydrodynamics (SPH) method is also a good candidate for treating primary atomization, thanks to its convective nature and its explicit treatment of the interface. It has shown good capability for treating primary atomization [START_REF] Hoefler | Multiphase flow simulations using the meshfree smoothed particle hydrodynamics method[END_REF]. Thus, another objective in this thesis is to apply this coupled approach to the coupling of SPH with a Finite Volume method.

We refer throughout the rest of the document the inner zone as Zonal Domain (ZD) and the outer zone as Global Domain (GD).

Outline of the thesis

The present document is composed of five chapters, excluding this introduction chapter. They are organized as follows.

Chapter 2 -Finite volume method

Chapter 2 is an introduction to the main numerical method used in this work, Finite Volume (FV) method. The FV notations correspond to those commonly used by the OpenFOAM R community. The discussion covers spatial, temporal and equation discretization as well as velocity-pressure coupling in incompressible formalism.

Chapter 3 -A zonal method for incompressible two-phase flows

Chapter 3 constitutes the core of the present thesis where the developed hybrid numerical method, that divides the flowfield into two zones, is presented. It is decomposed as follows.

• At the beginning, a literature review of Adaptive Mesh Refinement and Domain Decomposition Methods is given. These domain coupling techniques are closely related to the work realized in this thesis.

• Then, the two numerical models that will be combined by the hybrid method, i.e. a VOF model and a ELSA model, are detailed. It starts with the respective governing equations, that are discretized with the finite volume formalism, and ends with their respective solver algorithms.

• Next, the proposed numerical strategy, that combines the two previous solvers is detailed. A detailed algorithm is shown.

• The strategy is then validated on two two-dimensional test cases: a liquid-air jet and a rising bubble problem. A parameter study is performed on each parameter of the hybrid solver. Influences of the divergence-free and mass conservation corrections are investigated.

• Finally, the parallelization of the solver is detailed and validated.

Chapter 4 -Coupling SPH with finite volume

Chapter 4 is a preliminary extension of the previously detailed hybrid strategy by using SPH instead of the FV method in the zonal domain. Single phase and laminar flows are here considered. It is decomposed as follows.

• At the beginning, the Smoothed Particle Hydrodynamics discretization is introduced. The Weakly Compressible SPH formalism is detailed.

• Following, a literature review of existing works about SPH-FV coupling is given.

• Then, the single-phase SPH solver that has been developed in OpenFOAM R library is validated on two test cases: a Poiseuille flow and a laminar plane jet in a coflow.

• Next, the proposed strategy, that combines the SPH and the FV solvers together, is detailed. The coupling structure is similar to the FV/FV coupling, the interpolation processes here defer.

• Finally, this method is tested on the plane jet in a coflow configuration.

Chapter 5 -Application to numerical simulation of primary atomization

Chapter 5 described the application of the FV/FV two-phase zonal method on an airblast atomizer configuration. Comparisons of the numerical results are made with experimental data, scalability tests of the parallel solver are performed, and comparisons with a single model solver are discussed.

Chapter 2

Finite volume method

Introduction

The grid-based Eulerian method so-called Finite Volume (FV) method, one of the most employed discretizing technique in Computational Fluid Dynamics (CFD), is described in this part. This method is based on discretization of the integral form of governing equations over each control volume. Some quantities in the governing equations are turned into face fluxes and evaluated at the control volume faces. Because the flux entering a given volume is identical to that leaving the adjacent volume, mass and momentum are therefore conserved at the discrete level. This inherent conservation property is what make FV method a powerful method in CFD compared to Finite Element and Finite Difference methods. It is also easy to apply a variety of boundary conditions to the geometric domain, for modeling inlet flows, outlet flows, walls or atmospheric conditions. This section will present the basis of the FV method, applied to incompressible single phase Navier Stokes equations. It presents also the specificities inherent to OpenFOAM R Finite Volume code that has been used during this thesis.

OpenFOAM R is a multi-dimensional open-source software for continuum mechanics problems, including CFD. The C++ library allows the development of new solvers and functionalities by the research community and industrials. For instance, advanced boundary conditions and subgrid scale models for Large Eddy Simulation (LES) [START_REF] Piscaglia | Towards the les simulation of ic engines with parallel topologically changing meshes[END_REF] have been implemented in this software, as well as dynamic mesh handling [START_REF] Montorfano | An extension of the dynamic mesh handling with topological changes for les of ice in openfoam R[END_REF].

The reader is referred to the work of Jasak [START_REF] Jasak | Error Analysis and Estimation for the Finite Volume Method With Applications to Fluid Flows[END_REF] which is one of the researchers at the origin of OpenFOAM R 's FV implementation and to the books of Ferziger and Peric [START_REF] Joel | Computational methods for fluid dynamics[END_REF] and Versteeg and Malalasekera [START_REF] Henk | An introduction to computational fluid dynamics: the finite volume method[END_REF] for further and in-deep reading about the FV method.

Integral Form

Starting point for computational procedures in the FV method is a transport equation for a scalar quantity φ:

∂ρφ ∂t + ∇ • (ρφU ) = ∇ • (Γ∇φ) + Q φ . (2.1)
This transport equation 2.1 is composed of four different terms: A transient term ∂ρφ ∂t , a convection term ∇•(ρφU ) where U is the velocity field convecting φ, a diffusion term ∇•(Γ∇φ) where Γ is a diffusivity coefficient, and a source term Q φ . It is then integrated over a three-dimensional fixed-in-time domain Ω:

Ω ∂ρφ ∂t dΩ + Ω ∇ • (ρφU ) dΩ = Ω ∇ • (Γ∇φ) dΩ + Ω Q φ dΩ . (2.2)
Generalized Gauss' theorems will be directly applied in next derivations, involving these identities,

Ω ∇ • a dΩ = ∂Ω dS • a , ( 2.3
)

Ω ∇φ dΩ = ∂Ω dSφ , ( 2.4
)

Ω ∇a dΩ = ∂Ω dSa , (2.5)
where a is a vector, ∂Ω the boundary of domain Ω and dS an infinitesimal surface element with associated outward pointing normal to ∂Ω.

Applying Gauss's divergence theorem (Eq. 2.

3), integrated transport equation 2.2 may be written as follow:

∂ ∂t Ω ρφ dΩ + ∂Ω dS • (ρφU ) = ∂Ω dS • (Γ∇φ) + Ω Q φ dΩ . ( 2.6)
Convection and diffusion terms thus become surface flux terms, evaluated at the boundaries ∂Ω of the domain. This transformation has important consequences on the properties of the FV method, one of which is that it renders the method conservative. This integral form (Eq. 2.6) is valid both for the entire flow domain Ω and for a small Control Volume (CV), i.e. at the discrete level. A two-dimensional example of a control volume is given in figure 2.1. To obtain an algebraic equation for a particular CV, it consists to approximate surface integrals (see section 2.3), volume integrals (see section 2.4) and time derivative term (see section 2.7). These approximations are called discretization.

The accuracy of the discretization method depends on the assumed variation of the scalar function φ = φ(x, t) in space and time around the point P considered as the centroid of the considered CV, located at x P . The variation can be evaluated through Taylor series expansion in space,

φ(x) = φ P + (x -x P ) • (∇φ) P + 1 2 (x -x P ) 2 : (∇ 2 φ) P + 1 3! (x -x P ) 3 :: (∇ 3 φ) P + ... + 1 n! (x -x P ) n ::: (∇ n φ) P , (2.7)
and time, where φ P = φ(x P ), φ t = φ(t) and operation ::: is the inner product of two n th rank tensors resulting in a scalar.

φ(t + ∆t) = φ(t) + ∆t ∂φ ∂t t + 1 2 ∆t 2 ∂ 2 φ ∂t 2 t + 1 3! ∆t 3 ∂ 3 φ ∂t 3 t + ... + 1 n! ∆t n ∂ n φ ∂t n t , (2.8)
The order of accuracy of a discretization method depends on the truncation error when neglecting terms in Taylor Series expansion equations (2.7) and (2.8).

Approximation of surface integrals

Two terms in the integrated transport equation 2.6 require integration over the surface of a CV: convection term and diffusion term.

Integration over the CV domain of the quantity φ is the summation of the integration over each face of the quantity φ:

∂Ω dSφ = f S f dSφ . (2.9)
To calculate the surface integral in this equation exactly, it is necessary to know the integrand f everywhere on the considered surface S e . This information is not available, since only the nodal (CV center) values of φ are calculated, thus an approximation must be introduced. This is done using two levels of approximation:

• The integral is approximated in terms of the variable values at one or more locations on the cell face;

• the cell-face values are approximated in terms of the nodal (CV center) values (by interpolation).

CHAPTER 2. FINITE VOLUME METHOD

Three approximation methods of surface integrals are shown below for a face e owned by a control volume with centroid P inside a two dimensional Cartesian grid (see figure 2.1).

• Midpoint rule: 2 nd order of accuracy,

Se

dSφ S e φ e .

(2.10)

It is the most-commonly used surface integral approximation in the FV method, since it depends only on one point, limiting further necessary interpolations.

Justification of the order of accuracy

Starting from face integral form of second order truncated Taylor series expansion of φ in space (Eq. 2.7):

Se dSφ = Se dS[φ e + (x -x e ) • (∇φ) e ] = Se dS φ e + Se (x -x e ) dS = 0 •(∇φ) e = S e φ e .
(2.11)

The second integral in the last equation is equal to zero because the point e is the center of the face.

• Trapezoid rule: 2 nd order of accuracy,

Se

dSφ S e (φ ne + φ se ) 2 .

(2.12)

• Simpson rule: 3 rd order of accuracy,

Se

dSφ S e (φ ne + 4φ e + φ se ) 6 .

(

2.13)

To obtain values at the center of the face (φ e ) or/and in the corners (φ ne and φ se ), interpolations with the nodal values are necessary (see section 2.5).

Approximation of volume integrals

Source and transient terms in equation 2.6 (or any term not in a conservative form) require integration over the volume of a CV. Two approximations with second and fourth order of accuracy are shown below [START_REF] Joel | Computational methods for fluid dynamics[END_REF]:

• Central Point Rule : 2 nd order of accuracy Ω φ dΩ φ P V P .

(2.14)

Interpolation practices 39

Justification

Starting from volume integral form of second order truncated Taylor series expansion of φ in space (Eq. 2.7):

Ω φ dΩ = Ω [φ P + (x -x P ) • (∇φ) P ] dΩ = φ P Ω dΩ + Ω (x -x P ) dΩ = 0 •(∇φ) P = φ P V P .
(2.15)

The second integral in the last equation is equal to zero because the point P is the centroid of the control volume. This approximation is the most-commonly used one for (i) its simplicity and (ii) its compact stencil.

• Bi-quadratic shape function: 4 th order of accuracy

Ω φ dΩ V P (16φ P + 4φ n + 4φ w + 4φ e + 4φ s + φ se + φ sw + q ne + φ nw ) 36 .
(2.16)

Compared to central point rule, accuracy of this approximation is increased with the number of points involved in the stencil (9 points are considered in 2D). One drawback of such approximation is the computational cost of this non-compact stencil when the system is implicitly solve.

To obtain values at the face centers and at the control volume corners, interpolations of nodal values are necessary. It is treated in the following part.

Interpolation practices

As previously mentioned, for approximation of surface integrals or for approximation of volume integrals, interpolation with the nodal values are necessary in order to obtain values located at the center of the faces and in the corners. Interpolation schemes in OpenFOAM R software can be chosen by the user prior the simulation, for convection term and diffusion terms of the momentum equation. Two typical schemes are upwind and linear, respectively first order and second order accurate. They are detailed below:

• Upwind Interpolation or Upwind Differencing Scheme (UDS): 1 st order of accuracy

φ e = φ P if (U • n) e > 0 , φ E if (U • n) e < 0 .
(2.17)

Discretization of spatial terms

Here, following OpenFOAM R formalism, the convection and diffusion terms in transport equation will be discretized using midpoint rule (Eq. 2.10) as surface integral approximation and the source term in transport equation will be discretized using central point rule (Eq. 2.14) as volume integral approximation.

Convection term

Convective term in transport equation 2.6 is expressed as the summation of the integration over each face of the term (ρφU ):

∂Ω (ρφU ) dS = f S f dS • (ρU φ) f , (2.21)
where f is the sum over a series of flat faces f bounding CV. Applying mid point rule (Eq. 2.10) on RHS in equation 2.21 gives,

f S f dS • (ρU φ) f = f S • (ρU φ) f , = f S • (ρU ) f φ f , = f F m φ f , (2.22)
where F m is the mass flux through the face:

F m = S • (ρU ) f . (2.23)
The calculation of this face flux uses interpolated values of ρ and U from cell centroids to face centers. Equation 2.22 also requires face values for transport variable φ. A convection differencing scheme is employed in that way. It insures the boundedness of φ.

Central Differencing Scheme (CDS) also called linear scheme and Upwind Differencing Scheme (UDS) are two convection differencing scheme that have been described respectively in equations (2.18) and (2.17). Despite its first order, UDS respects boundedness of the field, which is not the case with CDS which can causes unphysical oscillations in the solution. Blended differencing schemes represent an attempt to preserve both boundedness and accuracy of the solution. It is a linear combination of UDS (Eq. 2.17) and CDS (Eq. 2.18):

φ f = (1 -γ) (φ f ) U D + γ (φ f ) CD . (2.24)
The blending factor γ, 0 ≤ γ ≤ 1, determines how much numerical diffusion will be introduced. Perić [START_REF] Joel | Computational methods for fluid dynamics[END_REF] proposes a constant γ for all faces of the mesh. For γ = 0 the scheme reduces to UDS and inversely, for γ = 1, it reduces to CDS.

Diffusion term

The diffusion term in transport equation 2.6 is expressed as the summation of the integration over each face of the term Γ∇φ:

∂Ω dS • (Γ∇φ) = f S f dS • (Γ∇φ) f . (2.25)
Applying mid point rule (Eq. 2.10) on RHS in equation 2.25 gives,

f S f dS • (Γ∇φ) f = f S • (Γ∇φ) f , = f Γ f S • (∇φ) f , (2.26)
If the mesh is orthogonal, i.e. if vectors d and S in figure 2.2 are collinear, it is possible to use the following expression: An alternative would be to calculate the cell-centered gradient for the two cells sharing the face as, (∇φ

S • (∇φ) f = |S| φ N -φ P |d| . ( 2
) P = 1 V P f Sφ f , ( 2.28)
to interpolate it to the face with a linear interpolation method (Eq. 2.18),

(∇φ) f = λ f (∇φ) P + (1 -λ f ) (∇φ) N , ( 2.29)
and finally to dot-product it with S.

Although both of the above described methods are the same order of accuracy, first method has a weaker truncation error so it is preferred. However, first expression must be corrected in the case of non-orthogonality mesh which is the most common case in CFD. More details about non-orthogonality are given in following section 2.6.2.1 and section 2.13.2 about the mesh quality.

Non-orthogonality

To take in account non-orthogonality (see figure 2.3), we shall split the product S • (∇φ) f into two parts:

S • (∇φ) f = ∆ • (∇φ) f orthogonal contribution + k • (∇φ) f non-orthogonal contribution , ( 2.30)
where the two vectors ∆ and k are decompositions of vector S:

S = ∆ + k . (2.31)
∆ is chosen to be parallel with d (see figure 2.34). Thus, equation 2.27 may be applied on orthogonal contribution term in equation 2.30:

S • (∇φ) f = |∆| φ N -φ P |d| + k • (∇φ) f .
(2.32) (∇φ) P expression (Eq. 2.28), face interpolation (Eq. 2.29) and k expression (Eq. 2.31) are used to compute the non-orthogonal contribution term (also called cross diffusion) in equation 2.32. The remaining unknown is the amplitude of vector ∆. Many possible decompositions exist. Let us shows three of them, the third one (over-relaxed approach) being the one use in OpenFOAM R solvers.

• Minimum correction approach: The decomposition of S, seen in figure 2.3, is done in such a way to keep the non-orthogonal correction in equation 2.32 as small as possible, i.e. to keep k amplitude as small as possible, by making ∆ and k orthogonal: • Orthogonal correction approach: This approach, shown in figure 2.34, keeps the contribution of the orthogonal term the same as it is with an orthogonal mesh. In other words, vector amplitude of ∆ is equal to the one of the surface vector |∆| = |S|: • Over-relaxed approach: In this approach, seen in figure 2.35, the more the face is non-orthogonal, the more the importance of the orthogonal term is. This approach has been found to be the most stable even when the grid is highly non-orthogonal.

∆ = d • S d • d d . ( 2
∆ = d |d| |S| . ( 2
∆ = S • S d • S d . (2.35)
To summarize, the diffusion flux at a face element of a non-orthogonal grid cannot be written solely in terms of the values at the nodes φ P and φ N around the face. A term that accounts for non-orthogonality has to be added. It is indeed computationally cheaper to considerer nonorthogonal term as an explicit source term than to include a large stencil approximation into the system matrix. As a drawback, it implies iterating a few times for solving a matrix in order to update the explicit non-orthogonal term with last known values. For a fully orthogonal mesh, it is non necessary to iterate, while for a highly non-orthogonal mesh, two iterations should be necessary. This non orthogonal term is also denoted in the literature by "cross diffusion".

Source terms

Source terms, such as S φ (φ) in transport equation 2.1, can be a general function of φ. Before discretization, the term is linearized:

Q φ (φ) = φQ I + Q E , ( 2.36)
where Q I and Q E may depend on φ. Considering equation 2.36 and using central point rule (Eq. 2.14), integrated source term in equation 2.6 is expressed as:

Ω S φ dΩ = V P φQ I + V P Q E . (2.37)
It can be noted that a discretized source term with central point rule does not need additional informations from neighbor cells, thus interpolations. All informations are stored in cell P .

Temporal discretization

For unsteady problems, a transient term is considered in the transport equation 2.1. It is thus a partial differential equation with an initial condition: [START_REF] Joel | Computational methods for fluid dynamics[END_REF]. We shall then apply some of them to the discretized transport equation integrated in space (Eq. 2.6).

∂(ρφ) ∂t = -∇ • (ρφU ) + ∇ • (Γ∇φ) + S φ = f (t, φ(t)) ; φ(t 0 ) = φ 0 . ( 2

Methods for initial values problems in ODEs

φ n+1 = φ n + f (t n , φ n )∆t . (2.41)
Implicit of Backward Euler method: 1 st order of accuracy

φ n+1 = φ n + f (t n+1 , φ n+1 )∆t . (2.42)
Midpoint rule: 1 st order of accuracy

φ n+1 = φ n + f (t n+1/2 , φ n+1/2 )∆t . (2.43)
Trapezoid rule or Crank-Nicholson method: 2 nd order of accuracy

φ n+1 = φ n + 1 2 [f (t n , φ n ) + f (t n+1 , φ n+1 )]∆t .
(2.44)

Temporal discretization

• Predictor-Corrector Methods

The predictor-corrector methods consist in using a (m -1) th order method as a predictor and a m th order method as a corrector. As an example below, an explicit predictorcorrector using explicit Euler as a predictor and explicit trapezoid rule as a corrector:

Predictor φ * = φ n + f (t n , φ n )∆t . (2.45) Corrector φ n+1 = φ n + 1 2 [f (t n , φ n ) + f (t n+1 , φ * )]∆t .
(2.46)

• Multipoint Methods

Adams-Bashforth, 2 nd order of accuracy:

φ n+1 = φ n + ∆t 2 [3f (t n , φ n ) -f (t n-1 , φ n-1 )] . (2.47)
Adams-Bashforth, 3 rd order of accuracy:

φ n+1 = φ n + ∆t 12 [23f (t n , φ n ) -16f (t n-1 , φ n-1 ) + 5f (t n-2 , φ n-2 )] . ( 2.48)
Adams-Moulton, 3 rd order of accuracy:

φ n+1 = φ n + ∆t 12 [5f (t n+1 , φ n+1 ) + 8f (t n , φ n ) -f (t n-1 , φ n-1 )] .
(2.49)

• Runge-Kutta Methods 2 nd order of accuracy:

φ * n+1/2 = φ n + ∆t 2 f (t n , φ n ) , φ n+1 = φ n + ∆tf (t n+1/2 , φ * n+1/2 ) .
(2.50)

4 th order of accuracy:

φ * n+1/2 = φ n + ∆t 2 f (t n , φ n ) , φ * * n+1/2 = φ n + ∆t 2 f (t n+1/2 , φ * n+1/2 ) , φ * n+1 = φ n + ∆tf (t n+1/2 , φ * * n+1/2 ) , φ n+1 = φ n + ∆t 6 [f (t n , φ n ) + 2f (t n+1/2 , φ * n+1/2 ) + f (t n+1/2 , φ * * n+1/2 ) + f (t n+1 , φ * n+1 )] .
(2.51)

Application to the transport equation

In previous paragraph, we have shown finite difference methods for discretizing transient term.

We now apply three of them to the transport equation:

• Explicit discretization (Eq. 2.41),

• Implicit Euler method (Eq. 2.42),

• Crank-Nicholson method (Eq. 2.44).

We start from the integrated equation 2.6:

∂ ∂t Ω ρφ dΩ + ∂Ω dS • (ρφU ) + ∂Ω dS • (Γ∇φ) = Ω Q φ dΩ .
It is integrated in time from t n to t n+1 and all previous term discretizations are applied:

t n+1 tn   ∂ρφ ∂t V P + f F m φ f - f Γ f S • (∇φ) f   dt = t n+1 tn (V P φQ I + V P Q E ) dt .
(2.52)

• Explicit discretization (Eq. 2.41) or forward Euler method, which is first oder of accuracy, gives an explicit expression for determining new values φ n+1 P :

φ n+1 P = φ n P + ∆t ρ P V P   - f F m φ n f + f Γ f S • (∇φ n ) f + V P φ n P Q I + V P Q E   , (2.53) with S • (∇φ n ) f = |∆| φ n N -φ n P |d| + k • (∇φ) n f , ( 2.54)
and

φ n f = f x φ n P + (1 -f x )φ n N . (2.55)
It is no longer necessary to solve a system of linear equations. But it is unstable if the Courant number Co is greater than unity [START_REF] Courant | Uber die partiellen differenz-gleichungender mathematischen physik[END_REF]. The Courant number is defined as:

Co = U f • d ∆t .
(2.56)

• Implicit Euler method (Eq. 2.42), also first order accurate, uses new time-level cell values for face-values, gradient and source term:

φ n+1 P = φ n P + ∆t ρ P V P   - f F m φ n+1 f + f Γ f S • ∇φ n+1 f + V P φ n+1 P Q I + V P Q E   ,
(2.57) with

S • ∇φ n+1 f = |∆| φ n+1 N -φ n+1 P |d| + k • (∇φ) n f , ( 2.58)
and

φ n+1 f = f x φ n+1 P + (1 -f x )φ n+1 N . ( 2
φ n+1 P = φ n P + 1 2 ∆t ρ P V P   - f F m φ n f + f Γ f S • (∇φ n ) f + V P φ n P Q I + V P Q E   , + 1 2 ∆t ρ P V P   - f F m φ n+1 f + f Γ f S • ∇φ n+1 f + V P φ n+1 P Q I + V P Q E   .
(2.60)

Crank-Nicholson method is unconditionally stable but does not guarantee the boundedness of the solution.

Solution of linear equation systems

The result of the discretization process described in the previous sub parts is a system of algebraic equations. Let us introduce two types of system: explicit and implicit.

Explicit system

In previous section, explicit Euler method (equation 2.41) for temporal discretization has been applied on transport equation 2.53:

φ n+1 P = φ n P + ∆t ρ P V P   - f F m φ n f + f Γ f S • (∇φ n ) f + V p φ n P S I + V p S E   . (2.61)
We may rewrite this equation as an algebraic equation, for every CV, in this form: Let us take as an example of implicit algebraic equation, the discretized transport equation 2.57 using an implicit Euler temporal discretization method (Eq. 2.42):

a P φ n+1 P + N a N φ n N = B P , ( 2
φ n+1 P = φ n P + ∆t ρ P V P   - f F m φ n+1 f + f Γ f S • ∇φ n+1 f + V p φ n+1 P S I + V p S E   .
(2.64)

It produces an algebraic equation, for every CV, in this form:

a P φ n+1 P + N a N φ n+1 N = B P , (2.65)
and the following system of algebraic equations for all CVs of the discretized domain:

[A] [φ] = [B] , (2.66)
where [A] is a sparse matrix, with coefficients a P on the diagonal and a N off the diagonal. To solve this system, efficient methods are needed. There are two categories:

• Direct methods as Gauss Elimination, LU Decomposition or Cyclic reductions. They give the solution of the system of algebraic equation in a finite number of arithmetic operations. This number approximatively scales with the cube of the number of unknowns, making them prohibitively expensive for large systems.

• Iterative methods as Jacobi, Gauss-Seidel(GS), Successive Over-Relaxation (SOR) or Biconjugate Gradient Stabilized Method (BiCGSTAB). They start with an initial guess and then continue to improve the current approximation of the solution until a defined tolerance criterion is reached.

Boundary conditions

The solution of a problem within the domain Ω depends on the governing equations representing a particular phenomenon and on the boundary conditions given at the ∂Ω boundary. These boundary conditions represent the interaction of the phenomenon inside the domain with the universe outside it. Boundary conditions can take many forms, but most of them can be divided into two types:

• Dirichlet prescribes the value of the dependent variable on the boundary and is therefore referred to as "fixed value".

• von Neumann prescribes the gradient of the variable normal to the boundary and is therefore referred to as "fixed gradient".

The discretization of spatial terms excluding source terms previously discussed involve the sum over faces f of the face interpolate φ f or the face gradient ∇φ f . The numerical boundary condition treatment is invoked when the sum over faces includes boundary faces. Therefore, a numerical boundary condition must be specified on every boundary face and for each dependent variable. Some additional parameters are required in the following part. Figure 2.6 shows a control volume P . One of its faces coincides with the boundary of the space domain. This face is labeled b. The vector between the cell center P and the center of the boundary face is denoted d and its component normal to the boundary face is d n . In the following, it is assumed that the boundary condition specified is valid for the whole face. The numerical implementation of fixed value and fixed gradient boundary conditions is described next, along with zero gradient and inlet-outlet boundary conditions:

• Fixed Value boundary condition

A fixed value prescribes the value of φ at the face b to be φ b . This has to be taken into account in the discretisation of the convection and diffusion terms on the boundary face.

-Convection term: According to equation 2.22, the convection term is discretized as:

f f dS • (ρU φ) f = f F m φ f . (2.67)
It is known that the value of φ on the boundary face is φ b . Therefore, the convection term for the boundary face is:

(F m ) b φ b , ( 2.68)
where (F m ) b is the mass face flux at the boundary b.

-Diffusion term: According to equation 2.26, the diffusion term is discretized as:

f f dS • (Γ∇φ) f = f Γ f S • (∇φ) f . (2.69)
The face gradient at b is calculated from the known face value and the cell center value:

S • (∇φ) b = |S| φ b -φ P |d n | , ( 2.70)
because S and d n are parallel.

• Fixed Gradient boundary condition

In the case of a fixed gradient boundary condition, the dot-product of the gradient and the outward pointing unit normal is prescribed on the boundary:

S |S| • ∇φ b = g b . (2.71)
-Convection term: The face value of φ is calculated from the value in the cell center and the prescribed gradient: (2.74)

φ b = φ P + d n • (∇φ) b , φ b = φ P + |d n |g b . ( 2

• Zero Gradient boundary condition

The zero gradient boundary condition is a fixed gradient boundary condition with g b = 0 and the discretization practices outlined above are applied.

• Inlet-outlet boundary condition

The inlet-outlet boundary condition is a mixed boundary condition, between a fixed value boundary condition and a zero gradient boundary condition. The mode of operation is determined by the sign of the volumetric flux F across the boundary faces. When the flux is positive, i.e. going out of the domain, a zero gradient boundary condition is applied. When the flux is negative, i.e. going into the domain, a fixed value boundary condition is applied.

Variable arrangement on the grid

Primitive scalar quantities or properties φ as pressure, temperature or species are generally stored at the cell centers. Concerning velocity components, their locations can be either at the same location (collocated arrangement) or at the face centers (staggered arrangement).

• Collocated Arrangement This arrangement was out a favor for a long time for incompressible flow computation due to the difficulties with pressure-velocity coupling and the occurrence of oscillation in the pressure. When improved pressure-velocity coupling algorithms were developed in the 1980's, the popularity of the collocated arrangement began to rise. One of them is Rhie-Chow decoupling scheme [START_REF] Cm Rhie | Numerical study of the turbulent flow past an airfoil with trailing edge separation[END_REF]. It consists to subtract the pressure gradient from the guess flux term F * = S • U * . Guessed velocity U * is a velocity computed with momentum balance without contribution of the pressure term. Also, evaluating the pressure gradient at the faces is based on pressure values at nodes. The benefit of these two tricks is that pressures checker-board oscillations are avoided.

• Staggered Arrangements With staggered arrangements, velocity components are stored on face centers. Staggered grids show two advantages:

-A natural coupling between velocities and pressure. For incompressible flows, it avoids oscillations occurring by solving the Poisson pressure equation with collocated arrangement.

-It avoid interpolations for obtaining velocity values on cell faces when computing convective fluxes or viscous fluxes. However, most of modern codes use a collocated storage since all variables are stored at the same place, making it easier to handle different control volumes.

Discretization of the Navier-Stokes equations

Previously, it has been shown how to discretize a generic transport equation. Here, Navier-Stokes equations are considered and we aim to apply previous discretization principles to the momentum and continuity equations. Several assumptions are made to express and close the governing equations:

• The fluid state is isothermal on the whole domain and during the whole computation.

Thus, energy equation is not considered.

• The fluid is incompressible, its density does not vary in time and in space: ∂ρ ∂t = 0,∇ρ = 0. • The fluid is Newtonian.

• The flow is transient.

Based on these assumptions, continuity and momentum equations, are expressed as:

∇ • U = 0 , (2.75) ∂U ∂t + ∇ • (U ⊗ U ) = ∇ • (ν∇U ) - ∇P ρ .
(2.76)

Since we consider incompressible flows, for a shorter formalism, the absolute pressure P is replaced by the kinematic pressure p = P ρ :

∂U ∂t + ∇ • (U ⊗ U ) = ∇ • (ν∇U ) -∇p . (2.77)
From momentum equation 2.77, two major points are put forward:

• Non-linearity of the convective term ∇ • (U ⊗ U ),

• The pressure-velocity coupling.

Regarding non-linearity of the convective term, there are two possible solutions, either use a solver for non-linear systems, either linearize the convection term. It is much cheaper regarding computational cost and simpler to linearize the convection term than solving a non-linear system. Linearization is the solution chosen in OpenFOAM R solvers. It consists to base the face flux F on the last known solution of velocity U at the previous time-step. This flux should

CHAPTER 2. FINITE VOLUME METHOD

also satisfy continuity equation 2.75 and therefore can only be lagged during the simulation.

Ω ∇ • (U ⊗ U ) dΩ = ∂Ω dS • (U ⊗ U ) , = f f dS • (U ⊗ U ) f , = f (S • U f ) U f , = f F U f , = a P U P + N a N U N , (2.78)
where F = S • U f represents face flux, a P are the diagonal coefficients of the discretization matrix and a N the off-diagonal ones. F is function of U .

Regarding pressure-velocity coupling, since no evolution is given for the pressure, it is necessary to devise a method to obtain a discretized equation which allows to solve the pressure.

Derivation of the pressure equation

In order to derive the pressure equation, we shall start from a semi-discretized form of the momentum equation:

a P U P = H(U ) -∇p . (2.79)
In the spirit of the Rhie and Chow procedure [START_REF] Cm Rhie | Numerical study of the turbulent flow past an airfoil with trailing edge separation[END_REF], the pressure gradient term is not discretized at this stage. This equation is obtained from the integral form of the momentum equation using the surface and volume discretization. The H (U ) term regroups advective term, diffusive term and source terms including the source part of the transient term. It is expressed as:

H(U ) = - N a N U N + U n ∆t , ( 2.80)
where index n denotes previous time step.

Continuity equation 2.75 is discretized as:

∇ • U = f S • U f = 0 , ( 2.81)
and momentum equation 2.79 is rearranged in order to obtain an explicit equation for U P :

U P = H(U ) a P - 1 a P ∇p . (2.82)
From previous equation 2. [START_REF] Ann S Almgren | A conservative adaptive projection method for the variable density incompressible navierstokes equations[END_REF], an expression for face velocity U f can be obtained by interpolating it from cell centroids to face centers:

U f = H(U ) a P f - 1 a P f (∇p) f . (2.83)

Discretization of the Navier-Stokes equations 53

This gives a base for face flux calculation by dot-producting it with surface area:

F = S • U f . (2.84)
Now, using this last expression of face velocity (Eq. 2.83), it can be substituted into continuity equation 2.81 to obtain the following form of the pressure equation:

∇ • 1 a P ∇p = ∇ • H(U ) a P , (2.85) f S • 1 a P f (∇p) f = f S • H(U ) a P f . (2.86)
Thus, we have a discretized system for U and p in the case of incompressible Navier-Stokes equations:

U P = H(U ) a P - 1 a P ∇p . (2.87) f S • 1 a P f (∇p) f = f S • H(U ) a P f , (2.88)
where cell-centered U is solved explicitly while cell-centered pressure p is solved implicitly. The face flux F is calculated using equation 2.83:

F = S • U f = S •   H(U ) a P f - 1 a P f (∇p) f   . (2.89)
Theses fluxes are conservative, when pressure equation 2.88 is satisfied.

Pressure-velocity coupling

Consider the discretized form of the Navier-Stokes system, equations (2.87) and (2.88). The equations form shows linear dependence between velocity and pressure gradient. This is called velocity-pressure coupling. A special treatment is required in order to solve the system. Two main methods are considered in literature:

• Simultaneous algorithms: the system is solved considering a single matrix. Such procedures involve a very large matrix, several times larger than the number of computational points and thus a great computational cost, which limits its use in standard CFD codes. However, it shows better convergence properties than the segregated methods presented below.

• Segregated approaches (SIMPLE algorithm [START_REF] Suhas | A calculation procedure for heat, mass and momentum transfer in three-dimensional parabolic flows[END_REF], PISO algorithm [START_REF] Raad | Solution of the implicitly discretised fluid flow equations by operatorsplitting[END_REF]): the equations are solved in sequence, in a loop where the convergence to a solution in pressure and velocity is sought after. Such algorithms are very popular and preferred to simultaneous ones for their lighter memory cost.

PISO algorithm for transient flows: icoFoam solver

Let's illustrate PISO algorithm from segregated approaches with icoFoam, a solver inherent to the OpenFOAM R library. This solver deals with transient incompressible laminar Navier-Stokes equations, without contribution of a source term such as gravity. This is one of the most basic incompressible solver in OpenFOAM R library and thus is a perfect simple example. The PISO loop consists of an implicit momentum predictor followed by a series of implicit pressure solutions and explicit velocity corrections. Each step of the algorithm will be described mathematically and linked to its corresponding part in the C++ code of icoFoam solver. The corresponding version is 5.0. Algorithm is summarized in figure 2.7.

(1) Velocity predictor:

As a first and optional step, an estimation of velocity U * at next time step is guess based on pressure field p n and velocity face flux F n at known time t n , using semi-discretized momentum equation,

U * = U n - ∆t V f F n U * f + ∆t V f νS • (∇U * ) f -∆t∇p n . (2.90)
This predicted velocity is not divergence-free, i.e. ∇ • U * = 0. The same momentum equation written in semi-discretized form is:

U * P = H(U * ) a P - 1 a P ∇p n . ( 2.91)
Corresponding code in icoFoam solver is:

fvVectorMatrix UEqn ( fvm::ddt(U) + fvm::div(phi, U) -fvm::laplacian(nu, U) ); if (piso.momentumPredictor()) { solve(UEqn == -fvc::grad(p)); } This predictor step is optional: on the one hand, it helps to get closer to velocity solution at next time-step but on the other hand, it has a cost to solve implicitly a matrix. Performing this step thus depends on the studied flow configuration.

(2) Computing pseudo-velocity:

The so-called pseudo-velocity is computed without pressures and source terms, at index m,

Ũ P = H(U m ) a P , ( 2
Ω ∇ • Ũ = b F = 0 , (2.94)
where b stands for all boundary faces of the computational domain Ω. This adjustment is made by multiplying each adjustable outlet flux with a corrector coefficient.

Corresponding code is:

adjustPhi(phiHbyA, U, p);

(5) Implicit pressure direct solution:

Poisson equation for pressure (Eq. 2.88) is implicitly solved for computing pressure at iteration index m,

f S • 1 a P f (∇p m ) f = f S • H(U m ) a P = f F . ( 2
U n+1 = U m , F n+1 = F m , p n+1 = p m , t n → t n+1 .
(2.98)

Discretization of the Navier-Stokes equations 57

New time step between t n and t n+1

(1) (Optional) Solve implicitly approximate velocity N denotes the total number of unknowns in the discretized problem. ε is the stopping criterion or accuracy for iterative solvers.

U * = f (U * , U n , F n , ∇p n ), else U * = U n U m = U * , ∇p m = ∇p n (2) Compute intermediate velocity Ũ = f (U n , U m ) (3) Compute intermediate face flux F = f ( Ũ ) (4)
F m = f ( F , ∇p m ) Next time step U n+1 = U m , F n+1 = F m , ∇p n+1 = ∇p m ,

Multigrid concept

Multigrid method consists to solve a given problem on a hierarchy of grids with different cell sizes, generally with a refinement ratio of two. Fundamental idea is that high frequency errors decline rapidly with iterative methods like Gauss-Seidel at the opposite of low frequency errors that decline with a much slower rate. On the finest mesh, low frequencies will be seen as low frequencies on a coarser grid. The goal of the multigrid algorithm is thus to increase the lowest frequencies by interpolating (restricting) the error from a fine block to a coarse block. Block are superimposed, of same size but with different refinements. Let us develop the mathematical background of the concept. The multigrid algorithm is based on two principles: error smoothing and coarse grid correction. First, one needs to define the residual of a system solved by an iterative method. Consider the following system of equations arising from the finite volume conservation discretization of a conservation equation on a flow domain (Eq. 2.66):

[A] [φ] = [B] , ( 2
[A] [Y ] = [B] -[R] .
(2.100)

Multigrid methodology 59

The difference between the real solution vector [φ] and the intermediate solution vector [Y ] is defined as the error vector [E]:

[E] = [φ] -[Y ] . (2.101)
Substracting equation 2.100 from equation 2.99 gives the following relationship between the error vector and the residual vector:

[A] [E] = [R] . (2.102)
This last equation system will be used to calculate, using an iterative method, the error vector at any stage stage of the iteration process. The residual vector [R] is obtained by rearranging equation 2.100:

[R] = [B] -[A] [Y ] . (2.103)
Iterative matrix form of equation 2.102 is written as:

[E] m+1 = [M ] [E] m + [C] , (2.104)
where m + 1 and m are iteration number, [M ] the iteration matrix depending on [A], [R] and a chosen iterative method (Jacobi, Gauss-Seidel,...) and [C] a constant vector depending uniquely on [A] and [R].

Properties of the iteration matrix [M ] determine the rate of error propagation, hence, the rate of convergence. They depend on the iterative technique, mesh size, discretization scheme etc. It has been established with the mathematical behavior of the matrix that the solution error components with a range of wavelengeths that are a few multiples of the mesh size (socalled short wavelengths or high-frequency components) decrease rapidly in a few iterations. However, long wavelengeths or low-frequency components decay very slowly as the iteration count increases.

Hence the principle of the multigrid process: increase mesh size so that the long wave lengths on the previous fine mesh become shorter on the next coarser mesh and decrease more rapidly in a few iterations. Transfer of informations from a fine to a coarse mesh are done by restriction. Recurrence of information from coarse to fine mesh by prolongation.

• Typical restriction operators are volume averaged. In a multigrid process, the information transferred through restriction is the residual vector [R].

• Typical prolongation operators are bilinear interpolation. In a multigrid process, the information transferred through prolongation is the error vector [E]. The generated values on the fine mesh after prolongation are called prolongated error vector [E] . On the fine mesh, the so-called coarse grid correction is then applied:

[Y ] improved = [Y ] + [E] .

Twogrid procedure

As an illustrative and relatively simple example, the procedure of a two-stage multigrid (or twogrid) is described below:

•

Some multigrid cycles

In order to improve the solution further, different cycles of coarsening and refinement are used.

A typical multigrid scheme is the V-cycle shown in figure 2

Mesh

Types of meshes

In general, a geometric domain may be discretized using either a structured grid or an unstructured grid system.

In a structured mesh, three dimensional elements are defined by their local indexes (i, j, k). Every interior cell in the domain is connected to the same number of neighboring cells that can be identified using their indexes. In 3D, for instance, a cell will be connected to 6 neighbors. This allows for lower memory usage since topological information is embedded in the mesh structure through the indexing system. It is called an implicit topological information. This made structured grid the favorite type of mesh at the beginning of finite volume and finite element developments, when memory capacities were low [START_REF] Moukalled | The finite volume method in computational fluid dynamics[END_REF]. However, a structured grid system suffers from a limited geometric flexibility. Additional flexibility in the generation of structured meshes can be achieved by employing multiple blocks to define the geometry, with a structured mesh generated for each block independently from other blocks.

Unstructured grids offer more flexibility in meshing a domain both in terms of element/cell types that can be used (hexahedron, tetahedron, prism or polyhedron) and in terms of where the elements can be concentrated. This flexibility costs, however, more complexity and memory storage. In an unstructured mesh, topological information is no longer implicit as in structured mesh but explicit. It is based on connectivity tables and geometric entity numbering, stored in memory. Connectivity tables link together cell to faces, face to owner, face to neighbor, cell to cells, etc. In OpenFOAM R software, which uses an unstructured grid system, each face owns an owner cell and a neighbor cell. The direction of the normal to the surface points toward neighbor cell. Sign of incoming and outcoming flux into a cell depend on this normal direction.

Thus, for computing a gradient, following finite volume discretization,

∇φ = 1 V P   f Sφ f   , (2.105)
the RHS term is split into sums over owned and neighboring faces:

∇φ = 1 V P   owner Sφ f - neighbor Sφ f   .
(2.106)

In addition to topological data, the finite volume mesh stores information about its geometric entities, such as cell volume, face areas, cell centroids, face centers, distance between owner and neighbor centroids, etc.

A third type of grid, so-called overlapping grids, is the combination of two or more grids to cover an irregular domain. One can combine for instance rectangular, cylindrical, spherical or non-orthogonal grids near bodies with structured grid in the rest of the solution domain. This method remedy to the flexibility issue of structured grids while keeping its good mesh quality and memory requirements. The disadvantage of this approach is that the programming and coupling of the grids can be complicated. It is also difficult to maintain conservation at the interfaces, and the interpolation process may introduce errors or convergence problems if the solution exhibits strong variations near the interface [START_REF] Joel | Computational methods for fluid dynamics[END_REF].

Mesh quality

The mesh quality can be conclusively determined based on the rate of convergence, the solution precision, the CPU time required and the grid independence result. Some criteria allow also to quantify and measure the suitability of the mesh. Let's detail some of the most important, i.e. the orthogonality, the skewness, the aspect ratio and the smoothness. The mesh orthogonality is the angular deviation of the face vector S, located at the face center f , from the vector d connecting the two cell centroids P and N . An illustration is shown in figure 2.10 with a deviation of 27 • . This orthogonality affects discretization of the diffusion 2.13 Mesh 63 term, as it has been treated in part 2.6.2, since it is necessary to add an explicit non-orthogonal correction term. This correction term is treated as a source term when solving the algebraic equations. A consequence is that the boundedness of the solution cannot be guaranteed. On the other hand, the non-orthogonal correction is usually small compared to the implicit part of the diffusion term. It is therefore reasonable to treat it through the source term [START_REF] Jasak | Error Analysis and Estimation for the Finite Volume Method With Applications to Fluid Flows[END_REF].

Orthogonality

P N f d S 27 •
The mesh orthogonality also affects the discretization of the pressure gradient in the Poisson pressure equation. Indeed, a source term treats the non-orthogonal part of the pressure gradient.

As a consequence, it is necessary to solve iteratively the Poisson pressure equation to account for the mesh non orthogonality. The more severe is the non-orthogonality, the more important is the number of iterations [START_REF] Joel | Computational methods for fluid dynamics[END_REF].

Skewness

The mesh skewness is the deviation of the vector d that connects the two cell centroids P and N . The deviation vector is represented with δ i and f i is the point where the vector d intersects the face f . The measure of the skewness, denoted sk, can be done following different manners. In OpenFOAM R tools, it is the ratio between the magnitude of the vector δ i and the magnitude of the vector d:

sk = |δ i | |d| . ( 2.107)
An illustration is shown in figure 2.11 with a skewness of 0.27, which is in a reasonable range lower than unity.

Skewness affects the interpolation of the cell centered quantities to the face center f . Indeed, mid point rule (Eq. 2.10) allows to approach surface integral terms as convection and diffusion terms by means of values located at the face centers:

f dSφ = Sφ f . (2.108)
The value φ f is obtained by linear interpolation from the points P and N around the face. This interpolation actually gives the value of φ in the point f i , which is not necessary in the middle of the face. A skewness correction shall be applied in interpolation with the following relation:

φ f = φ f + (∇φ) f • δ i . (2.109)

Aspect ratio

Mesh aspect ratio (AR) is the ratio between the longest side ∆x and the shortest side ∆y. Large AR smear gradients in the largest direction. It affects also the convergence of the solvers.

As an example, for a uniform 2D grid with a constant aspect ratio of 10 : 1 between ∆x and ∆y, , Gauss Seidel and MultiGrid-Gauss Seidel solvers performances are considerably deteriorated [START_REF] Joel | Computational methods for fluid dynamics[END_REF].

Smoothness

Smoothness, also known as expansion rate, defines the transition in size between contiguous cells. Large transition ratios between cells add diffusion to the solution. It affects particularly more cell-centered FV methods than staggered FV methods [START_REF] Moukalled | The finite volume method in computational fluid dynamics[END_REF]. Ideally, the maximum change in mesh spacing should be less than 20%.

Chapter 3

A zonal method for incompressible two-phase flows

Introduction

As stated in introduction, regarding the atomization process, the capture of the interface with large scale destabilization on the one hand and the computation of a vaporizing dispersed spray on the other hand need very different physical and numerical models to be correctly captured by any simulation. Therefore, the objective of this thesis is to address this "multiphysic" issue of the atomization process by developing an hybrid numerical method that divides the flowfield into two zones: a inner zone dedicated to capture the interface and high velocity gradients and a outer zone for the rest of the field, to follow less steep flow gradients. In the inner zone, so-called in this thesis Zonal Domain (ZD), an Interface Capturing Method (ICM) of type Volume-Of-Fluids (VOF) will be employed. In the outer zone, namely Global Domain (GD), a sub-grid or diffuse interface model of type Euler Lagrangian model for Spray and Atomization (ELSA) will be utilized. The criteria have been stated in the introduction: Each zone must be as independent as possible from the other one, with its own numerical and discretization schemes; the resolution in ZD is higher than in GD, i.e. the grid is refined in ZD.

Following this statements, a question arise: How to couple these two domains ? In this chapter, we address this question after. A literature review of multi-domain techniques will be given, in which we distinguish two main types of techniques:

• Adaptive Mesh Refinement (AMR) and more particularly patch and block-based AMR.

• Domain Decomposition Methods (DDM) in which we may distinguish three types of layout decompositions: patched grids, overlapping grids and zonal grids.

In a second part, the discretization and algorithms of the two employed two-phase flows methods, VOF and ELSA, are detailed. Third, we propose a strategy to couple ZD and GD, based on a combination of different concepts, among which are subcycling in time AMR and zonal grid DDM. Fourth, the strategy is tested and validated on two 2D test cases, a rising bubble FLOWS problem and a liquid-air jet. Fifth and finally, the parallelization of the coupled solver is detailed and validated.

Literature review of multi-domain techniques

Adaptive Mesh Refinement (AMR)

The quality of results in CFD is generally judged by the invariance of solutions with further mesh refinement. This approach is non optimized for engineering practice. In certain cases, a coarse mesh, that is just sufficient to describe the main geometrical properties of the computational domain, has already a large number of elements. Any further uniform refinement would lead to a configuration whose size would surpass the available computer resources.

It is thus necessary to refine in regions of interest. Meshing strategies are usually based on a subjective judgment, such as "more cells in the boundary layer" or "more cells in the primary atomization zone", etc., and work is needed to make the refinement process more objective, user-independent and, as a consequence, more efficient.

Adaptive Mesh Refinement (AMR) methods dynamically refine the mesh to capture sharp discontinuities and steep gradients according to the flow dynamic. A mesh broadening operation is also applied in areas with weak variations of the flow properties. Apart from the minimization of the number of grid cell that reduces the computational cost, a major advantage is the automation of the procedure that ease the meshing work. To do so, cells to be refined are tagged based on a refinement criteria.

This refinement criteria can be based on a specific variable or its gradient. For instance, in two phase flows problems when using VOF method, setting refinement criteria on both volume fraction gradient and curvature allows to better capture liquid/gas interface and its characteristics. In turbulent problems, setting this criterion on velocity gradient helps to better capture vorticities [START_REF] Fuster | Simulation of primary atomization with an octree adaptive mesh refinement and vof method[END_REF]. In some combustion problems, the flame front is the criterion (temperature, heat release, chemical activity, high vorticity [START_REF] Bell | Numerical simulation of a laboratory-scale turbulent v-flame[END_REF]). The rapid variations of quantities occurring in this production zone have to be solved with suitable accuracy. Typical mesh size necessary to catch the flame reaction zone is 10 µm, while the size of a combustion engine is of the order of 10cm. Hence, the recourse to AMR is clearly pertinent in combustion problems. A detailed multi-level AMR algorithm for flame front tracking is given in the work of Haldenwang and Pignol [START_REF] Haldenwang | Dynamically adapted mesh refinement for combustion front tracking[END_REF].

More generally, independently of the flow pattern, a common criterion consists in an estimated truncation error. In one of the first AMR paper, Berger and Oliger [START_REF] Marsha | Adaptive mesh refinement for hyperbolic partial differential equations[END_REF] proposed Richardson extrapolation, an error estimate method based on Taylor series expansion on two different meshes, to compute this criterion.

After each time iteration, each cell of the mesh is checked, and based on the refinement criteria, is tagged or not for further refinement, or in the opposite way, for coarsening. After tagging cells in regions of interest (see figure 3.1-(a)), refining them can be done by different manners. Two main categories of AMR methods can be distinguished:

• Adaptive methods, that use a unique mesh with local enrichment.

• Multi-level methods, that use separated blocks or patches. Refinement can be performed in space as well as in time.

We describe these two families in next subsections.

Adaptive methods

Adaptive methods or Adaptive Local Mesh Refinement (ALMR) allow the grid spacing and/or discretization schemes to respond to the local length scales of the flow. There are three categories of adaptive methods: r-refinement, p-refinement and h-refinement:

• r-refinement or moving grid method: Cells are moved or stretched but not added or deleted. It is referred to also as grid-point redistribution.

• p-refinement or adaptive order method: The order of accuracy of the discretization schemes is changed locally in the grid. It increases the stencil of tagged elements and allows to increases the rate of convergence. On the other hand, it produces larger matrices.

• h-refinement or local grid refinement method: Cells are subdivided into two or more subcells. It is also referred as cell-based AMR. FLOWS

In cell-based AMR, as proposed and developed for example by Power and co-workers [START_REF] Kenneth G Powell | Adaptive-mesh algorithms for computational fluid dynamics[END_REF][START_REF] Darren | An adaptively refined cartesian mesh solver for the euler equations[END_REF][START_REF] Zeeuw | A quadtree-based adaptively-refined Cartesian-grid algorithm for solution of the Euler equations[END_REF], each cell may be refined individually as shown in figure 3.1-(b) and is stored using a tree data structure (quadtree in two dimensions, and octree in three dimensions). This tree structure is flexible, readily allows for the local refinement of the mesh by keeping track of the computational cell connectivity as new grid points are generated by the refinement process and an efficient parallelization structure.

Cell-based AMR has proven its effectiveness on the atomization process simulation: the Gerris code from Popinet [START_REF] Popinet | An accurate adaptive solver for surface-tension-driven interfacial flows[END_REF] have been applied to the jet disintegration problem, using a VOF method [START_REF] Fuster | Simulation of primary atomization with an octree adaptive mesh refinement and vof method[END_REF][START_REF] Agbaglah | Parallel simulation of multiphase flows using octree adaptivity and the volume-of-fluid method[END_REF]. In [START_REF] Xue | Disi spray modeling using local mesh refinement[END_REF][START_REF] Xue | Development of adaptive mesh refinement scheme for engine spray simulations[END_REF][START_REF] Kolakaluri | A unified spray model for engine spray simulation using dynamic mesh refinement[END_REF], Xue Kong et al. applied similar scheme with a Euler-Lagrange method for engine spray simulations. Lucchini et al. [START_REF] Lucchini | Numerical investigation of the spray-mesh-turbulence interactions for high-pressure, evaporating sprays at engine conditions[END_REF] also coupled cell-based AMR with Euler-Lagrange method to investigate the spray-mesh-turbulence interactions for high-pressure engine atomization. More recently, Essadki et al. [START_REF] Essadki | Adaptive mesh refinement and high order geometrical moment method for the simulation of polydisperse evaporating sprays[END_REF] uses cell-based AMR for simulating a Taylor-Green evaporating spray.

Multi-level methods

In Multi-level methods, tagged cells are grouped together in so-called "patches" or "blocks", depending on the Multi-level variant, then refined to the next level of mesh refinement. For example, cells in a refined region at first level, can be tagged and refined to the second level with the generation of a new embedded region, that fully overlap previous "level 1" region. Refined regions are a series of level embedded one into another.

Multi-level methods was first proposed by Berger and Oliger [START_REF] Marsha | Adaptive mesh refinement for hyperbolic partial differential equations[END_REF] in 1984 with purpose to refine grids both in time and space and to reduce computational cost for solving hyperbolic partial differential equations. Each block is defined independently of the other blocks, with its own solution vector, storage, etc. As stated by Berger and Oliger [START_REF] Marsha | Adaptive mesh refinement for hyperbolic partial differential equations[END_REF], by keeping the grids independent, the Multi-Level algorithm can be viewed as a Domain Decomposition Method (DDM). DDM are methods that split the domain into several sub-domains and will be detailed in the next section. Most common variant, named Patch based mesh type method, consists of clustering tagged cells together into rectangular finer patches, superimposed to the coarser ones. This strategy is illustrated in figure 3.

1-(c).

Another method block-type AMR consists of dividing and coarsening the entire solution predefined blocks of groupings of cells, as shown in figure 3.1-(d). Block-based methods may more readily lend themselves to efficient and scalable parallel implementations via domain decomposition.

There are two approaches to solving the system of governing equations on a composite hierarchy of grids with different level refinements. The first one is to solve the system implicitly at each time step using a combination of multilevel operations. This approach requires that every level to be advanced with the same time step. This first approach has the drawback to apply a single time step all over the main domain. Even if the number of cells is optimized, the CFL condition in the finest cells may penalize the global time-step and hence the computational cost.

The second approach consists to advance each level independently with its specific time step:

∆t l+1 = (1/r t ) ∆t l , ( 3.1)
where r t is the time step ratio and superscripts () l+1 and () l respectively refer to fine and coarse levels. It can be referred to as time subcycled AMR or local time stepping techniques. This second approach requires no interlevel communication other than the supplying of data from a coarse level to be used as boundary conditions at the next finer level (prolongation step) and then to synchronize the data at different levels at some specified interval (restriction step) [START_REF] Ann S Almgren | A conservative adaptive projection method for the variable density incompressible navierstokes equations[END_REF].

Early works in this direction go back to Berger and Oliver [START_REF] Marsha | Adaptive mesh refinement for hyperbolic partial differential equations[END_REF] and Osher et al. [START_REF] Osher | Numerical approximations to nonlinear conservation laws with locally varying time and space grids[END_REF]. Then, Almgren et al. [START_REF] Ann S Almgren | An adaptive projection method for the incompressible euler equations[END_REF], Bell et al. [START_REF] Bell | A second-order projection method for the incompressible navier-stokes equations[END_REF], Martin et al. [START_REF] Daniel | A cell-centered adaptive projection method for the incompressible euler equations[END_REF]1] treated different important aspects of the Navier-Stokes solution, in particular the conservative aspects. Almgren et al. [START_REF] Ann S Almgren | A conservative adaptive projection method for the variable density incompressible navierstokes equations[END_REF] introduced the variable density computation, stressing the issue of conservation. Almgren et al. [START_REF] Ann S Almgren | A conservative adaptive projection method for the variable density incompressible navierstokes equations[END_REF] note that the solved governing equations performed best at CFL numbers approaching one. Thus, the use of sub-cycling allows to keep an optimal CFL level by level and improve accuracy of the numerical solution in comparison with non-subcycled AMR.

After computation of the finer levels and synchronization of the data, if solution on the unrefined part of the base grid is not re-computed, it is called a passive AMR method. At the opposite, if an additional elliptic solve is performed during synchronization, it is referred to as an active method. This method is more appropriate for elliptic problems in which a change of conditions in any region may affect the solution everywhere [START_REF] Joel | Computational methods for fluid dynamics[END_REF].

Multi-level techniques are typically applied on Cartesian grids, making easier the generation of blocks or patches with coincident boundaries.

Let us now examine in detail an algorithm of multilevel AMR scheme with sub-cycling in time.

Time sub-cycled multilevel AMR of Martin et al. [1]

We synthesize in this paragraph the multilevel AMR scheme proposed by Martin et al. [1] in 2008. We chose to explain this method since it is one of the most recent and detailed work about this type of time sub-cycling AMR algorithm. Other algorithm variants have been proposed by the same laboratory (Lawrence Berkeley National Laboratory, California) and extended to variable density flows [START_REF] Ann S Almgren | A conservative adaptive projection method for the variable density incompressible navierstokes equations[END_REF], two-phase flows [START_REF] Sussman | An adaptive level set approach for incompressible two-phase flows[END_REF], Euler equations [START_REF] Daniel | A cell-centered adaptive projection method for the incompressible euler equations[END_REF] and multiphase flows with parallelized CLSVOF method [START_REF] Sussman | A parallelized, adaptive algorithm for multiphase flows in general geometries[END_REF]. However, the two last ones do not use time sub-cycling schemes for the reason that the computational gain is not obvious when refining in time close to a liquid-gas interface.

As a reminder, the objective of this thesis is to develop a zonal method, in which the meshing work and the zonal domain generation are done prior to the computation by the user. Thus, the refining/coarsening process of Martin's algorithm is not detailed in this paragraph, focus is done on the multilevel update algorithm, that concerns us more.

The described adaptive algorithm is based on a Cartesian grid approach. It is block-based and, as previously mentioned, sub-cycled in time. Equations that are solved are the unsteady incompressible Navier-Stokes equations in three dimensions. Pressure-velocity coupling is solved with a projection method. The refinement ratio between two consecutive levels is 2 : 1.

After the different levels have been generated/deleted based on the given criterion, the multilevel update algorithm is proceeded. It can be summed up as following:

Level 0 Level 1 Level 2 (φ) n (φ) n+1 (φ) n (φ) n+ 1 r 1 (φ) n+1 (φ) n (φ) n+ 1 r 2 (φ) n+ 1 r 1 (φ)
• Each level l is advanced (solved) in time independently. The boundary conditions of the rectangular patch are supplied either from the underlying level l -1 through linear interpolation in time and space, either from physical domain boundaries. This step is repeated r times with time step ∆t l = (1/r) ∆t l-1 . We shall refer to this boundary condition supplying as a prolongation procedure, similarly to the Multigrid designation, since informations are transferred from the coarser to the finer grid. In the following, the operator P will refer to this prolongation procedure.

• After r advancements, data are synchronized between levels l and l -1. This step is two-way, i.e. data are averaged from levels l to l -1 and correction are interpolated from levels l -1 to l. This procedure involves thus both restriction operations and multilevel elliptic solves. Restriction processes consist in averaging operations from a finer grid to a coarser one. In the following, the operator R will refer to this restriction procedure.

Literature review of multi-domain techniques 71

Algorithm

Let us now go deeper in the details of the algorithm. The algorithm is illustrated with an example showing two levels of refinement in figure 3.2.

First, level 0 is entirely solved using global time step ∆t 0 . Then, finer level 1 is recursively resolved. This second step is decomposed into two subparts: First subpart is a prolongation P procedure: the boundary conditions at the coarse-fine interfaces of level 1 are supplied by level 0, through quadratic interpolation of level 0 solution. The boundary conditions consist of ghost cells lying outside interface. Dirichlet conditions as well as Neumann conditions are supplied by interpolations of neighbor level 0 values. More details about these conditions are given later. Then, in second subpart, level 1 is entirely resolved using a sub-cycled time step ∆t 1 = (1/r 1 ) ∆t 0 . At the end of the first level 1 time-step, finer level 2 is recursively resolved, in the same manner than previously for level 1.

At the end of a time-step at a given level, if some finer levels have been resolved, a synchronization step is performed. This process is split into four subparts, including two restriction procedures and two multilevels elliptic solves [1]:

• Reflux for conservation First subpart involves a face-centered restriction procedure R of the fine boundary fluxes, in order to compute the mismatches between the coarse and fine level fluxes along coarse-fine interfaces. Then, this mismatch is used to correct the solution along the coarse side of coarse-fine interfaces. This correction is explicit for non-diffusive scalars, implicit otherwise (an elliptic equation is solved on coarse level), and preserve conservation of mass and momentum.

Since time sub-cycling is performed, fine interface fluxes must be accumulated over the r time steps before being "restricted". Thus, the restriction process R is a time and face-averaged operation.

• Divergence free correction Second subpart of the synchronization aims to ensure that the velocity field is divergence-free in a composite sense (by considering all levels). It is necessary to solve an auxiliary elliptic Poisson equation to correct the whole solution. This equation is solved implicitly on all levels simultaneously, requiring linear interpolations at the coarse/grid interfaces for each iteration.

• Free-stream preservation correction Third subpart ensures that the free-stream is preserved. Free-stream preservation means that a constant scalar fields with no source term should remained unchanged independently of the grid refinement patterns and the velocity field. Let us illustrate this with an auxiliary advected scalar field Λ whose governing equation and initial conditions are:

∂Λ ∂t + ∇ • (U Λ) = 0 , Λ (x, t = 0) = 1 . (3.2)
When Λ is different from its initial value, a velocity correction is computed from the Λ mismatch by solving an elliptic multilevel equation. FLOWS

• Coarse solution correction Fourth subpart of data synchronization involves a cellcentered restriction procedure R. Cell-centered fields at the new time in levels l and l + 1 do not correspond. Thus, this mismatch is corrected by a cell-centered averaging procedure from the fine grid to the coarse one.

The concept of the synchronization step is similar in other multilevels algorithms [START_REF] Ann S Almgren | A conservative adaptive projection method for the variable density incompressible navierstokes equations[END_REF][START_REF] Sussman | An adaptive level set approach for incompressible two-phase flows[END_REF][START_REF] Daniel | A cell-centered adaptive projection method for the incompressible euler equations[END_REF][START_REF] Sussman | A parallelized, adaptive algorithm for multiphase flows in general geometries[END_REF]; the main differences are the ordering of the subparts and the way to correct divergence free and free-stream preservation. In the algorithm of Almgren et al. [START_REF] Ann S Almgren | A conservative adaptive projection method for the variable density incompressible navierstokes equations[END_REF], the elliptic equations are solved on a single level at a time, interpolating corrections to finer levels.

Boundary condition interpolations

In the paper of Almgren et al. [START_REF] Ann S Almgren | A conservative adaptive projection method for the variable density incompressible navierstokes equations[END_REF], detailed description of the coarse-fine interfaces updating through interpolations are given.

In their algorithm, boundary conditions are implemented by filling "ghost cells" outside each block, similarly to [1]. These ghost cells are filled by copying from other fine grids, where possible, otherwise by interpolating from underlying coarse grids or imposing physical boundary conditions, as appropriate. The boundary conditions consists of either Neumann either Dirichlet data. For Neumann data, the extrapolation procedure uses the given normal derivative from the coarser grid and internal values in the fine grid to define a value in the ghost cell. For Dirichlet data, the extrapolation procedure uses the neighbor values in the coarser grid to define a value in the ghost cell. The interpolation procedure operates in two steps:

• Tangential interpolation along interface (in one and two directions respectively in two and three dimensions).

• Normal interpolation between the intermediate points and the patch fine cells to obtain the value in the ghost cell.

Domain Decomposition Methods (DDM)

Introduction

Before detailing the Domain Decomposition Methods (DDM), let us remind three major challenges in CFD:

(i) The physics of the flow itself (e.g. turbulence).

(ii) Geometrical complexity of realistic configurations.

(iii) Maintaining required numerical accuracy with good computational economy.

Decomposition of the physical domain into several sub-domains coupled together may be an effective solution to these three items.

For instance, regarding the point (ii), complex geometries often occur in aerospace field, e.g. flow around an aircraft or flow between a wing and a nacelle. Generating a suitable mesh around such bodies is a challenging task. A first approach that has been investigated by researchers to address this issue consists to use an unstructured grids composed of triangular and tetrahedrons control volumes, respectively in two and three-dimensions. Discretizing the flow by such elements provides flexibilities in grid generation. An hybrid multiblock grids will also provide the possibility to use refined cell layers near the bodies. However, this meshing approach remains a cumbersome task costing engineering time in order to obtain a mesh of quality, i.e. with low skewness, aspect ratio and non-orthogonality values(see section 2.13.2). Another alternative regarding complex geometries is the DDM. With such approach, one or more body fitted meshes are generated and coupled together with an underlying mesh that covers the whole domain.

Thus, the domain decomposition method (DDM) lies on two principle elements: the subdivision of the computational domain and the communication among the sub-domains.

The DDM divides the flow region into simpler sub-domains within which grids are independently or semi-independently generated using existing grid generation schemes (structured, curvilinear, unstructured,...). An advantage of such method is that the flow regions requiring refinement can be isolated from the main domain into different sub-domains, addressing the point (iii) previously mentioned. In addition, the decomposition method enables the use of different partial differential equations and solutions methods in each sub-domain. For instance, in aerospace field, the Navier-Stokes equations can be used to investigate the domain near a body (a wing, wall, nacelle,...) where viscous effects are preponderant, while the Euler equations may be used in the far-field where convection dominates. This address the point (i). These two points, (i) and (iii), are precisely two of the criteria that our method aims to fulfill.

At last, DDM allows to solve faster a fixed size problem thanks to the block-processing technique: The solution domain is subdivided into sub-domains, each one being assigned to a given processor. Thus, the block-processing technique permits parallel computing. Since each processor needs data that resides in other sub-domains, exchange of data between processors is necessary.

Let us now consider the different type of interface layouts in DDMs.

Interface layouts

The second element of DDM to discuss, after the subdivision of the computational domain, is the communication between sub-domains. Communication, or data transference, between domain boundaries are accomplished by some type of interpolation method of either nonconservative or conservative nature. Each sub-domain can be connected to a neighbor zone with a simple patch (patched grids) or they can share a common region (overlapping grids). A last possibility is to define a grid that fully overlaps a larger region (zonal grid). These three topologies are illustrated in figure 3.3 and detailed there after.

Patched grids

Patched grids method employs disjoint sub-domains that share a simple interface or patch without overlapping. It was proposed by Rai [START_REF] Mohan | A conservative treatment of zonal boundaries for euler equation calculations[END_REF] for the finite difference method and then extended to the finite volume method by Walters et al. [START_REF] Walters | Aspects and applications of patched grid calculations[END_REF]. In such approach, neighboring FLOWS blocks with neat interfaces allow to have a better conservative description than, for instance, in overlapping grids method. Numerous works have exploited this conservative property [START_REF] Chen | Navier-stokes simulations for transport aircraft wing/body high-lift configurations[END_REF][START_REF] Zhang | Improvement to patched grid technique with high-order conservative remapping method[END_REF] and improved it [START_REF] Rinaldi | Flux-conserving treatment of nonconformal interfaces for finite-volume discretization of conservation laws[END_REF][START_REF] Horacio J Aguerre | Conservative handling of arbitrary non-conformal interfaces using an efficient supermesh[END_REF]. On the other hand, this method has more difficulties to handle complex geometries because of the interface constraint. In this thesis, this is not a concern since we consider atomization configurations with relatively simple geometry.

In context of atomization, a patch grid method has been used in the work of Zuzio et al. [START_REF] Zuzio | Numerical simulation of primary and secondary atomization[END_REF] for coupling an separated phase solver with a dispersed phase solver, respectively dedicated to the primary and the secondary atomization regions. This is very close to what is seek in this thesis. The coupling is however established only at the interface between the two domains and sub-cycling in time is not performed.

Overlapping grids

Overlapping grids method, also called Chimera method, has been introduced by Benek et al. [START_REF] Ja Benek | A flexible grid embedding technique[END_REF][START_REF] Pg Buningt | A 3-d chimera grid embedding technique[END_REF] in 1983. This method is used to perform simulations involving multiple bodies in relative motion and multiple grids that are overlapping. Within the overlap region, the grids communicate through data transference by an interpolation procedure. Grid embedding schemes allow the sub-domains to be non-disjoint so that one mesh may be embedded completely or partially within another. This procedure permits each sub-domain to be meshed independently with no requirements of continuous grid lines across boundaries.

Because each sub-domain grid is independent of another, grid generation task is greatly reduced for complicated flow regions. Each sub-domain mesh can be created using different grid generation techniques suitable for that particular domain. This is specially beneficial for sub-domains which require high grid densities, as previously mentioned.

Its development was also motivated by the possibility to refine selectively the mesh in regions of interest and to solve different flow models on each mesh. Benek et al. [START_REF] Ja Benek | A flexible grid embedding technique[END_REF][START_REF] Pg Buningt | A 3-d chimera grid embedding technique[END_REF] solve Navier-Stokes (NS) equations in near-wall areas and Euler equations in zones far from the walls. This NS/Euler hybrid approach have since been applied in numerous works [START_REF] Jee | Euler and navier-stokes simulations of helicopter rotor blade in forward flight using an overlapped grid solver[END_REF][START_REF] Ja Ekaterinaris | A zonal method for unsteady, viscous, compressible airfoil flows[END_REF][START_REF] Richard | A coupled euler/navier-stokes algorithm for 2-d unsteady transonic shock/boundary-layer interaction[END_REF]. In the context of multiphase flows, overlapping grids methods have been developed by Tu [START_REF] Tu | Computation of turbulent two-phase flow on overlapped grids[END_REF] to model complex turbulent two-phase flows with irregular geometries. It has been recently applied by Nguyen et al. [START_REF] Van-Tu Nguyen | Navier-stokes solver for water entry bodies with moving chimera grid method in 6dof motions[END_REF] on moving bodies entering into water or by Castro et al. [START_REF] Li | A pressure-velocity coupling approach for high void fraction free surface bubbly flows in overset curvilinear grids[END_REF] and Wan et al. [START_REF] Shen | Dynamic overset grids in openfoam with application to kcs self-propulsion and maneuvering[END_REF] about ship hydrodynamic problems. In [START_REF] Henshaw | Adaptive mesh refinement on overlapping grids[END_REF], a patch-based AMR is coupled with Overlapping grids method: One curvilinear grid fits the body and a Cartesian grid is used for the rest of the domain. In both grids, a multilevel AMR allows to refine them dynamically. This AMR/Overlapping grids combination is a remedy to the issue of patch-based AMR, i.e. only applicable in structured/curvilinear meshes.

Zonal grid

In some specific cases, a given zone can fully overlap a larger region. It is called the zonal grid method and can be seen as the superposition of a local grid and a global grid. It can also be seen as a variant of overlapping methods. It uses successive refinement of grids where a coarse grid solution constitutes the boundary conditions for the next finer grid level. It is similar to patch-structured AMR, the difference being that here grids are static and pre-defined by the user prior to the computational run.

In literature, it has been used to improve the resolution of near wall boundary layers in [START_REF] Khanna | Analysis of monin-obukhov similarity from large-eddy simulation[END_REF] and [START_REF] Manhart | A zonal grid algorithm for {DNS} of turbulent boundary layers[END_REF] using respectively LES and DNS. In these works, the purpose of adding a zonal refined grid to a global coarsen grid is to refine locally inside a wall boundary layer. A resulting configuration is shown in figure 3.4. Hybrid schemes with various turbulence models can also be used, as in the work of Richez et al. [START_REF] Richez | Near stall simulation of the flow around an airfoil using zonal rans/les coupling method[END_REF] where a Reynolds averaged Navier-Stokes (RANS) turbulence model is used in the main domain while LES describes the walls boundary layer. It has also been widely used in meteorological applications [START_REF] Ley | Forecasts of typhoon irma using a nested-grid model[END_REF][START_REF] Kurihara | Design of a movable nestedmesh primitive equation model[END_REF][START_REF] Sullivan | A grid nesting method for large-eddy simulation of planetary boundary-layer flows[END_REF] for refining the mesh inside high velocity gradient structures such as hurricanes.

Summary and discussion

In this section, different approaches from literature concerning multi-domain techniques were detailed. Special emphasis was placed on multi-level Adaptive Mesh Refinement methods because we identify a multi-domain strategy with sub-cycling in time as a possible candidate for the coupling of a fine local domain with a coarse global domain.

Among existing DDMs, the zonal grid topology shows the benefit of a pre-defined static grid placed in a region of interest and fully embedded in a global domain. Furthermore, DDMs allow to use different numerical and discretization method in each sub-domain, such as in overlapping methods.

These three mentioned characteristics will be used in the numerical coupling method detailed in section 3.4.

Let us now detail the two-phase flow solvers that will be coupled together.

Two-phase flow solvers

In this section, the two-phase flow solvers that will be coupled together are detailed. The first solver uses a VOF method to track the interface with a specific algorithm surface compression method [START_REF] Weller | A new approach to vof-based interface capturing methods for incompressible and compressible flow[END_REF] to limit numerical diffusion. It will be referred as the Resolved Interface (RI) solver in the following. As previously mentioned, the second solver does not consider any surface tension and since turbulent flows are considered, it can be shown that the turbulent diffusion flux term prevails in the primary phase volume fraction evolution. Thus, this solver will be referred as the Turbulent Diffusion Flux (TDF) solver.

Governing equations

Let's us consider a two-fluids flow with a high density fluid denoted 1 and a low density fluid 2. Both fluids are incompressible and non miscible. In the present work, phase 1 is taken as the reference fluid component, i.e. the primary phase. A volume fraction α is the VOF field, a scalar field representing the volume fraction of fluid 1,

α =      1 in fluid 1 0 in fluid 2 0 < α < 1 at the interface (3.3)
Considering incompressible flows, without mass transfer across the interfaces, the governing equations includes continuity:

∇ • U = 0 , (3.4)
where U is the velocity vector. The momentum balance is given by:

∂ρU ∂t + ∇ • (ρU U ) -∇ • (µ ef f ∇U ) = -∇P rgh + ∇U • ∇µ ef f + Q , (3.5)
where ρ is the density, which is calculated as presented in equation 3.10, and P rgh is the dynamic pressure defined as:

P rgh = P -ρg • x , ( 3.6)
where P is the pressure, g the gravity acceleration and x the position vector. The efficient dynamic viscosity term µ ef f = µ + ρν t is the sum of the molecular dynamic viscosity µ and the turbulent effects ρν t . The turbulent kinetic viscosity ν t is given by the chosen turbulence model. The source term Q includes the gravity acceleration g. Moreover, when a resolved interface between the two fluids is considered, the surface tension is added to Q. Then,

Q = Q D = -g • x∇ρ , Q I = -g • x∇ρ + f σ , ( 3.7)
where the subscript () D is specific to a turbulent diffusion flux solver and () I stands for a resolved interface modeling. In this last case, the surface tension f σ is applied at the interface position. This force is defined by:

f σ = σκ∇α I , (3.8)
where σ is the surface tension coefficient and, by defining n as the interface unit normal, then

κ = -∇ • n = -∇ • ∇α I |∇α I | , ( 3.9)
is the interface curvature.

The fluid density and viscosity are functions of the phase indicator α:

ρ = αρ 1 + (1 -α)ρ 2 , ( 3.10)
and

µ = αµ 1 + (1 -α)µ 2 . (3.11)
Density and viscosity in each separate phase 1 and 2 are considered constant.

Besides the mass and momentum equations, the VOF method requires to keep track of the volume fraction. This is performed by advecting the VOF field with the incompressible velocity field through the following equation:

∂α ∂t + ∇ • (αU ) = 0 . (3.12)
Equation 3.12 transports mixture properties and position of the interface. In case of a sharp interface, an interface capturing method is necessary to well define geometric characteristics of the interface and correctly compute body force surface tension in momentum equation 3.5.

Resolved interface (RI solver)

In the RI solver, a conservative form of equation 3.12 is exploited with an additional surface compressive term in order to keep the interface sharp [START_REF] Rusche | Computational fluid dynamics of dispersed two-phase flows at high phase fractions[END_REF]:

∂α I ∂t + ∇ • (U α I ) = -∇ • [U c α I (1 -α I )] compressive term , ( 3.13)
where the α I (1 -α I ) term enforces the compressibility term to be concentrated only at the interface region. Thus, it has little or negligible effect on the solution throughout the rest of the FLOWS domain. U c is a suitable velocity field selected to compress the interfacial region [START_REF] Berberović | Drop impact onto a liquid layer of finite thickness: Dynamics of the cavity evolution[END_REF], defined as a relative velocity between the two phases:

U c = min [C α | U |, max (| U |)] n , (3.14)
where the min operator is performed locally, at the faces surrounding the concerned cell and the max operator is performed globally, in the entire domain. The compressibility coefficient C α is usually of order 1. In this work, it was set to unity. As described by Rusche [START_REF] Rusche | Computational fluid dynamics of dispersed two-phase flows at high phase fractions[END_REF], the artificial compressive term of equation 3.13 provides interface straightening without the need to use an interface reconstruction method, with the advantage that the boundedness of α between 0 and 1 is respected.

Diffuse interface (TDF solver)

TDF solver exploits a filtered version of balance equation for the liquid volume fraction (Eq.3.12) with an additional term namely the turbulent diffusion liquid term:

∂α D ∂t + ∇ • (U α D ) = ∇ • R α turb. diff. liquid term . (3.15)
This turbulent liquid flux defined as R α = U α represents the turbulent transport of the liquid volume fraction induced by velocity fluctuations U . A widely exploited approach is based on a gradient closure approximation:

R α = ν t Sc t ∇α D , (3.16)
where Sc t is the turbulent Schmidt number equal to 0.7.

Discretized model equations

The discretized forms, using finite volume, of the transport equation are now proposed. Indeed the coupling between the two grids on which two different solvers are solved involves an exchange of information between the discrete parameters of each solver such as the faces fluxes or volume data. Thus, they are introduced in the following.

Momentum equation

The discretized form of momentum equation 3.5 is presented following the standard OpenFOAM R formalism:

V ∆t ρ n+1 U n+1 -ρ n U n + f (ρF ) n+1 U n+1 f = -V ∇(P rgh n ) + f µ n+1 ef f f S • ∇U n+1 f + f U n f S • ∇µ n+1 ef f f + V Q n , ( 3.17)
where () n and () n+1 superscripts identify instant t and t + ∆t, respectively. Subscript () f indicates the face values, interpolated between the volume center P and the considered neighbor cell center N (see figure 3.5). The cell volume is V and the volumetric flow rate through one of its faces f is defined as

F = S • U f , (3.18)
where S is the face normal vector.

Phase indicator

RI solver Transport equation for volume fraction α I (Eq. 3.13) can be semi-discretized as,

α n+1 I = α n I -∆t{∇ • [U α I + U c α I (1 -α I )]} , (3.19)
and it is fully discretized as,

α n+1 I = α n I - ∆t V f [F × α I,f + F c × α I,f (1 -α I,f )] , ( 3.20)
where F c is the compressive face flux,

F c = (U c ) f Ŝ . (3.21)
The magnitude of interface normal face vector Ŝ is defined as:

Ŝ = n • S = ∇α I |∇α I | • S . (3.22)
For the sake of clarity in following, the two terms present in RHS sum of equation 3.20 are grouped together into one global phase flux term namely F α,I :

F α,I = F × α I,f + F C × α I,f (1 -α I,f ) . (3.23)
TDF solver The transport equation for phase indicator α D is given by equation 3.15. In discretized form, it may be expressed as:

α n+1 D = α n D - ∆t V f    F α,D advective + F νt dif f usive    , ( 3.24)
where the turbulent diffusive phase flux F νt is defined as,

F νt = ν t Sc t f S • ∇α D,f . (3.25)
As for the RI solver, we introduce a phase flux term namely F α,D that accounts for the contribution of advection, the turbulent diffusion term of equation 3.24 being left aside in the next steps of the resolution:

F α,D = F × α D,f . (3.26) FLOWS

Segregated pressure-based solver

In this section a joint description is proposed for both RI and TDF solvers, the structure of which being very similar. Parts specific the resolved interface solver are highlighted by (RI) while parts specific to the turbulent diffusive flux solver are denoted (TDF) . RI and TDF solvers are existing methods, respectively interFoam and twoLiquidMixingFoam solvers, available in OpenFOAM R library, version 5.0. RI solver has been detailed in the thesis of Rusche [START_REF] Rusche | Computational fluid dynamics of dispersed two-phase flows at high phase fractions[END_REF] and studied for instance in [START_REF] Klostermann | Numerical simulation of a single rising bubble by vof with surface compression[END_REF][START_REF] Raees | Evaluation of the interface-capturing algorithm of OpenFoam for the simulation of incompressible immiscible two-phase flow[END_REF]. TDF solver is based on the Eulerian-Lagrangian Spray Atomization (ELSA) method from Vallet and Borghi [START_REF] Vallet | Modélisation eulerienne de l'atomisation d'un jet liquide[END_REF]. It is a single-fluid approach composed of two species. The modeling approach employed in this work is similar to the mixing of two miscible liquids, at the differences that here the mixing is only turbulent and the two species shows highly variable density. It thus justifies the use of the twoLiquidMixingFoam solver as TDF solver.

(1) Advection equation for the primary phase α is solved N αSC times with explicit sub time stepping: This time subcycling allows to ensure a better stability since an explicit resolution is carried out. In this work, N αSC is equal to 2. For each sub-cycle loop, equation 3.27 is solved recursively two times, to update F i α value. The MULES (Multidimensional Universal Limiter for Explicit Solution) [START_REF] Márquez | An extended mixture model for the simultaneous treatment of short and long scale interfaces[END_REF] limiter is used to integrate equation 3.27 to ensure boundedness of the solution.

α i+1 = α i - δt V f F α (α i ) , ( 3
At the end of each sub-cycle loop, the advective mass flux ρF , necessary in stages ( 4) and ( 5) when computing the momentum conservation equation, is computed at sub-cycle index i with following expression:

ρF i = F i α × (ρ 1 -ρ 2 ) f + F × (ρ 2 ) f . (3.28)
Finally, after the N αSC loops, the advective mass flux is computed by time-averaging previous sub-cycled mass fluxes:

ρF n+1 = i ρF i N αSC . ( 3
α n+1 D -α n D ∆t - α D,adv -α n D ∆t = f F n+1 νt .
(3.30)

Two-phase flow solvers 81

Once equation 3.30 is implicitly solved, turbulent diffusive mass flux F νt × (ρ 1 -ρ 2 ) is added to previous advective mass flux,

ρF n+1 = ρF n+1 + F n+1 νt × (ρ 1 -ρ 2 ) . (3.31)
(3) Update of mixture properties:

(3.1) Density and viscosity are then updated,

ρ n+1 = α n+1 ρ 1 + (1 -α n+1 )ρ 2 , ( 3.32
)

µ n+1 = α n+1 µ 1 + (1 -α n+1 )µ 2 . (3.33) (3.2) (RI) Curvature is also updated, κ = -∇ • ∇α n+1 I |∇α n+1 I | , ( 3.34)
(4) Solving the momentum predictor: This step is optional: it helps to get closer to velocity solution at n + 1 with an estimated velocity U * . It involves an implicit resolution which as a cost non negligible. Performing this step thus depends on the configuration. The solution is derived from pressure p n and velocity face flux F n fields at old known time t n . Thus, this predicted velocity is not divergence-free, i.e. ∇ • U * = 0. This will be corrected in next stage PISO loop.

Starting from semi-discretized momentum equation 3.17 and introducing matrix coefficients, one gets the following expression for U * :

U * = H(U * ) a P + -∇(P rgh n ) + Q a P , ( 3.35)
where H(U * ) regroups source terms of the transient, advective and diffusive terms:

H(U * ) a P = ρ n ρ n+1 U n - ∆t ρ n+1 V   f (ρF ) n+1 U * f   - ∆t ρ n+1 V   f µ n+1 ef f f S • (∇U * ) f + f U n f S • ∇µ n+1 ef f f   .
(3.36)

The source term expression depends on which model is used. In RI solver, it is expressed as:

Q I = -(g • x) (∇ρ n+1 ) + (σκ) f (∇α n+1 ) . (3.37)
and in TDF solver: Then, face interpolated source term multiplied by surface is added to this flux:

Q D = -(g • x) (∇ρ n+1
F = Fu + |S|Q f (a P ) f . ( 3
F m = F -S • 1 a P f ∇P m rgh f . ( 3.43)
(5.5) Explicit velocity corrector: Finally, velocity is explicitly computed by summing pseudo-velocity, pressure term at index m and source term,

U m = Ũ + 1 a P -∇P m rgh + Q . ( 3.44)
(5.6) After N corr loops in (5), velocity, face flux and dynamic pressure are updated as solution at index n + 1,

U n+1 = U m , F n+1 = F m , P n+1 rgh = P m rgh .
(3.45)

Numerical coupling method

83

(1) Explicitly solve advection equation of α, for N αSC subcycles.

(2) (TDF) Implicitly solve diffusion equation of α D .

(3) Compute density ρ and viscosity µ.

(4) (Optional) Implicitly solve predictor velocity U * .

(5) Solve PISO loop for N corr cycles. RI and TDF single grid solver algorithms are synthesized in figure 3.6, following same step numbering.

Numerical coupling method

Both numerical solvers described previously are classically used to resolve two-phase flows evolution on a single grid. Our objective is to use simultaneously both solvers on two different grids, thanks to a zonal grid methodology, with separate refinement in time and space. This new TPZ (Two-Phase Zonal) approach aims to use most of the positive features of some of the previously described methods in the literature review:

1/ Use the sub-cycling in time of the AMR to reduce the computational costs of the fine mesh zones.

2/ Adopt the coincident interfaces method from the patched grids approach for a better conservation of the flow properties between neighbor zones. Global domain (GD) is the main computational domain while Zonal Domain (ZD) is fully overlapped in GD. Communication from GD to interface Γ is done via prolongation P operator.

Communication from ZD field to underlying GD field is done via restriction R operator.

Depending on the local characteristics of the flow, it is then possible to use a particularly refined zonal grid making it possible to capture very high local gradients. A suitable solver will be applied to this grid which is interactively coupled to the larger, coarser grid.

In this section, this new solver is developed in the framework of the OpenFOAM R library. The methodology may be applied for any solver. However, in this work, the interface tracking (RI) solver used is interFoam while the diffusive (TDF) solver is twoLiquidMixingFoam.

Notations

Let's recall that in the following, the domains are referred as the Global Domain (GD) and the Zonal Domain (ZD). GD is the complete geometry to be studied while ZD is a local domain fully superimposed on a part of GD (Fig. 3.7). ZD mesh is finer than GD mesh, since its purpose is to capture physical process finer than the resolution of GD. The interface between ZD and GD is referred to as Γ.

3.4 Numerical coupling method 85

Subcycling in time

Specific time-step is defined for each domain: ∆t on GD and ∆τ on ZD. Then,

∆τ = 1 r t ∆t, (3.46)
where r t is the time-step ratio between ZD and GD. This ratio can be either fixed or adaptive for each iteration.

• Fixed time-step ratio r t is fixed when ∆t is fixed as well. In that case, r t is equal to the mesh refinement ratio r x between ZD and GD, which is the ratio between GD average cell size (∆x) GD and ZD average cell size (∆x) ZD :

r t = r x = (∆x) GD (∆x) ZD . ( 3
where face-computed Courant number Co is defined as ,

Co = S • U f S • d P N ∆t , ( 3.49)
with d P N = x P -x N the distance between owner cell center P and neighbor cell center N (see figure 3.5). ∆t n refers to the time-step at the previous GD iteration (∆t being the one at the current iteration), Co max = 0.5, ∆t max are user-defined parameters and λ 1 = 0.1 and λ 2 = 1.2 are two hard-coded factors in order to increase time-step gradually and avoid unstable oscillations. A provisional value ∆τ * for the zonal grid time step is determined with a similar equation adapted to ZD.

Using relation 3.48 provides values for GD and ZD time-steps in the current time loop, respectively ∆t and ∆τ * . Since the time-step ratio between the two domains is an integer, ZD time-step is adjusted to fulfill this requirement. First, the time step ratio is rounded to upper integer bound:

r t = f loor ∆t ∆τ * + 1 , ( 3.50)
where f loor(a) is a function to obtain the closest integer lower than a. Then, effective ZD time-step ∆τ is determined using equation 3.46.

Solver algorithm

The principle for one GD time-step is described as following and illustrated in figure 3.8. The details of the interpolation and correction steps are given later. We start from the solution on both domains at t = t n and seek to find solution at t n+1 = t n + ∆t: FLOWS

(1) Solve entirely GD, for one global ∆t time step, using single grid solver algorithm.

(2) Do following, r t loops:

(2.1) Prolongation step: Coupled boundary conditions of ZD, at the interface Γ, are updated based on interpolation in time and space of GD solution at time t n+1 .

(2.2) Solve entirely ZD, for one zonal ∆τ time step, using single grid solver algorithm.

(2.3) Go back to (2.1) until t n+1 is reached.

(3) Restriction step: ZD solution fields at t n+1 are transferred to GD cells through interpolation procedures.

Treatment of the zonal/global grid interface (step (2.1))

Values imposed on coupled boundary conditions of ZD, at interface Γ, are computed at step (2.1) of the TPZG algorithm. A coupled boundary conditions means that some of the values imposed at the patch are interpolated from GD internal field. The two types of coupled boundary conditions that are used will be detailed later. This interpolation process is called prolongation step, similarly to its denomination in Multigrid method [START_REF] Joel | Computational methods for fluid dynamics[END_REF]. An illustration of the process is given in figure 3.10-(a). Let's introduce the prolongation operator P(φ) that interpolates any variable φ from GD field to the zonal interface Γ. This operator combines the three following interpolation steps:

• (step 2.1.1) Interpolation from cell centroids to face centers in GD, r t is the time refinement ratio between ZD and GD. U : velocity field, P rgh : pressure field, α: primary phase field and φ: a transported scalar field. Subscript () n is index for time instant t and () n+1 stands for time instant t + ∆t after one time step. Single grid solver is either RI solver either TDF solver. between face flux value (which is mass conservative) and the scalar product of velocity vector with interface normal:

U f = Ū f + F |S| -Ū f • n f n f , (3.51)
where Ū f is a linear interpolation of the neighbor cell center values at face f (see figure 3.5) and n f the face normal vector,

n f = S |S| . ( 3

.52) FLOWS

In that way, by dot producting equation (3.51) with n f , one gets

U f • n f = F |S| . (3.53)
This approach ensures that an interpolated face velocity is coherent with the volumetric flux at this face.

Phase indicator:

Mass conservative approaches are considered for the phase indicator field interpolation.

It is thus interpolated differently depending on which single grid solver is used:

-(RI) An expression for face center data is derived from phase flux equation (3.23):

F α = F × α f + F r × α f (1 -α f ) . (3.54)
Equation (3.54) is rearranged to obtain the following expression:

α f = F α F + F r (1 -α f ) . ( 3
α f = ρF -F × ρ 2 -F ν,α × (ρ 1 -ρ 2 ) F × (ρ 1 -ρ 2 ) . (3.56)

Other variables:

As far as other cell centered variables are concerned (P rgh , k or ε), a linear interpolation between the neighbor cell centroids P and N is employed:

φ f = ωφ P + (1 -ω) φ N , (3.57)
where ω is the weighting factor for linear interpolation, defined as: (2.1.3) Previous variables from (2.1.2) are interpolated tangentially to the zonal interface Γ:

ω = |x f -x N | |x P -x N | . ( 3
φ n+k/rt = φ n + k r t φ n+1 -φ n , (3.59) with k ∈ [1, r t ].
We use left-skewed and right-skewed blended interpolation for its property to conserve mass fluxes and its 2 nd order accuracy [START_REF] Manhart | A zonal grid algorithm for {DNS} of turbulent boundary layers[END_REF]. An illustration of this interpolation procedure is shown in figure 3.9 with a space ratio r x = 2 : 1. For a face centered value φ f , blended left and right-skewed linear interpolation to point i is expressed as a function of φ f at face indexes I, I + 1 and I -1:

(φ f ) i = (φ f ) I + d I,i • d I,I+1 d I,I+1 • d I,I+1 (φ f ) I+1 + d I,i • d I,I-1 d I,I-1 • d I,I-1 (φ f ) I-1 , (3.60)
where d a,b is the vector between two points a and b.

For interface corners only and to ease implementation, a 1 st order interpolation scheme is used, namely the injection scheme [START_REF] Manhart | A zonal grid algorithm for {DNS} of turbulent boundary layers[END_REF]. It consists to associate ZD boundary face value with its nearest neighbor GD face value:

(φ f ) i = (φ f ) I . (3.61)
Boundary condition types at interface Γ Three types of boundary conditions are used at the zonal interface Γ and are detailed below. Their assignation to the field variables will be given later, depending on the considered numerical test.

(i) A coupled Dirichlet condition simply consists to impose an interpolated field quantity from GD to ZD interface Γ, by using the prolongation operator P previously defined.

(ii) A coupled inlet-outlet condition is a mixed Dirichlet-Neumann condition, which switches between a coupled normal gradient when the fluid flows out of ZD at a patch face, and a coupled Dirichlet, when the fluid is flowing into ZD. A coupled normal gradient is defined by P(∇ ⊥ φ), while a a coupled Dirichlet is defined by P(φ). Table 3.1 describes this boundary condition.

CHAPTER 3. A ZONAL METHOD FOR INCOMPRESSIBLE TWO-PHASE FLOWS

Coupled inlet-outlet boundary condition F Γ ≥ 0 (out of domain) apply P(∇ ⊥ φ) F Γ < 0 (into domain) apply P(φ) This approach allows to benefit of the accuracy of the fine mesh when information is leaving ZD. It will be used as a coupled boundary condition for phase indicator α and other transported scalars. It will also be used for velocity U when a coupled Dirichlet boundary condition (i) is used for pressure.

(iii) A Neumann gradient boundary condition is used for dynamic pressure P rgh , when a coupled Dirichlet boundary condition (i) is used for velocity. The following value ∇P rgh is updated when solving pressure equation at PISO step (6.3) with the following expression:

∇P rgh = (a P ) f F -U f • S |S| . (3.62)
F is calculated using expression (3.41) at PISO step (6.3).

Interpolation from zonal to global domain (step (3))

After resolution of the ZD solution over ∆t, part of the solution field is interpolated from ZD to GD, to correct the coarse solution at instant t n+1 (Fig. 3.7.). This step is numbered (3) in zonal solver algorithm and figure 3.8. This process is called restriction, similarly to its denomination in Multigrid method [START_REF] Joel | Computational methods for fluid dynamics[END_REF]. The cell centered restriction operator R P brings variables from a pack of fine cells in ZD to an overlapped coarser cell in GD. We denote by R P (φ) a standard cell centered variable on a domain after restriction operator has been applied. We use volume average for its simplicity and its conservative property. Volume average restriction operator is expressed as:

R P φ GD = i (φ i V i ) ZD i V ZD i , ( 3.63)
where subscript index () i denotes the subset of control volumes on ZD level, that forms the considered control volume on coarse GD level. An illustration of cell center restriction is given in figure 3.10-(b).

Similarly, face centered restriction operator R f brings variables from a group of fine faces of ZD to an overlapped coarser face in GD. Restriction of fine face fluxes consists to sum over the group each face flux value to get coarser face flux value. Flux summing restriction operator is expressed as:

R f F GD = i F ZD i , ( 3.64)
where subscript index () i denotes the subset of faces on ZD level, that forms the considered face on coarse GD level. An illustration of face center restriction is given in figure 3.10-(c). Fields concerned by the restriction step are:

• Velocity field U ,

• Phase indicator field α,

• Volumetric face flux field F ,

• Turbulent kinetic energy k and turbulent dissipation ε fields, when the case is turbulent and a k -ε RANS approach is used. FLOWS Both cell center and face center restriction operators are applied on any entity of global domain mesh that is covered by finer entities of zonal mesh. Thus, interpolation occurs on all covered cells and all covered faces in GD. Concerning covered faces, it includes also physical boundary conditions.

Treatment of global grid correction (step (4))

In previous restriction step, phase indicator α, velocity U , face flux F and transported scalar fields φ are interpolated from ZD to GD. Final step, numbered step (4) in solver algorithm 3.8, consists now to correct GD solution at time n + 1. It is similar to active AMR [START_REF] Joel | Computational methods for fluid dynamics[END_REF] where influence of local domain is spread over the entire global domain. The following steps are performed.

First, since volumetric face fluxes F have been interpolated from ZD to GD, it can be observed important continuity error at the interface between ZD and GD, because of flux mismatches.

It is crucial to correct GD F flux field to ensure a divergence free velocity, low continuity errors and to obtain a converged solution. We refer to this correction step as divergence free correction step. It consists to "smooth" the face flux field by solving a Poisson equation and to ensure divergence free constraint. A dummy pressure field P corr is resolved using following equation ,

∇ • 1 a P ∇P corr = ∇ • U , ( 3.65)
where a P are the diagonal coefficients of the system matrix. Equation (3.65) is expressed in discretized form as,

f S • 1 a P f (∇P corr ) f = f F . (3.66)
Then, face flux field is corrected with following relation:

F corr = F -S • 1 a P f (∇P corr ) f . (3.67)
This process will affect both face flux values in uncovered and covered parts of the domain, leading to different flux field in zonal and global domains. However, it has been noticed that influence of this correction on flux field is mainly focused outside covered region while fluxes in covered region are weakly corrected. In order to avoid any flux correction in the covered part, one could impose a zero pressure gradient, or also increase drastically weight coefficients 1/a P in dummy pressure matrix. One could also solve this Poisson equation at both levels to keep fine and coarse flux fields coherent. This requires a more complex algorithm and intergrid interpolations at each time step, which has a non negligible cost.

Second, it is important to take in account phase flux mismatch at the interface and to correct the α values in coarse cells along the interface Γ, to ensure mass conservation. We refer to this correction step as phase flux correction step. Coupled boundary conditions treatment in ZD imposes α values when flux is going in ZD and normal gradient when flux is going out. As a consequence, at the interface, phase fluxes in ZD does not match underlying phase fluxes in GD. The cell-centered restriction step will correct the α in the covered part of GD, but not in the coarse side of ZD interface. The current correction aims to correct α in these cells. To do so, a face-centered restriction of phase flux is operated at the interface. To explain this correction, we shall start from equation 3.20 for RI model and equation 3.24 for TDF model.

It is now expressed independently of the model:

α n+1 = α n - ∆t V f F α,o , (3.68)
where F α,o stands for the overall phase flux in each model, i.e. advective plus compressive fluxes in RI model and advective plus diffusive fluxes in TDF model. Now, one introduces similar conservation equation that takes in account the phase flux at the interface (F α,o ) Γ , after facecentered restriction , namely R f (F α,o ) Γ , and the corrected phase value at new instant α n+1 corr :

α n+1 corr = α n - ∆t V   f -1 F α,o + R f (F α,o ) Γ   , ( 3.69)
where f -1 stands for sum over all faces of the cell except the face underlying interface. Rearranging equation 3.69 and including equation 3.68, one obtains the following expression for α n+1 corr :

α n+1 corr = α n+1 - ∆t V R f (F α,o ) Γ -(F α,o ) Γ . (3.70)
Equation 3.70 is applied over all cells along the zonal grid interface Γ. In the case where α n+1 is equal to 0 or 1 in a given cell, boundedness of the corrected value α n+1 corr is ensured by a distribution of the overflow (> 1) or the lack (< 0) of liquid to the neighboring cells. This is known as the Robin Hood procedure [START_REF] Lawrence D Cloutman | A convective flux limiter for non-lagrangian computational fluid dynamics[END_REF].

Third and last, in case RI solver is used in GD, interface geometry properties, curvature and position, are corrected using new values of volume fraction field α.

Initialization of zonal fields

The global and zonal solvers are run and coupled together from the starting point of the simulation. Thus, initialization of zonal fields is identical to any CFD preprocessing: initial conditions are set up by the user prior to solving the computational domain. These conditions must be equal in both zonal and global domains. One can consider starting simulation with global solver only, then initialize and solve the zonal domain later in the simulation, as detailed in following paragraph.

Perspective of developments

Depending on the configuration, in order to save computational resources, the zonal-global coupling could be activated later in the simulation. It would start with the global coarse domain only, until a user-defined time from which starts the coupling with a fine zonal domain. In that case, mapping of solution between meshes will be necessary. This is a prolongation procedure of internal fields from coarse global mesh to fine zonal mesh. The mapping method proposed by Jasak in his thesis [START_REF] Jasak | Error Analysis and Estimation for the Finite Volume Method With Applications to Fluid Flows[END_REF] is a good solution for incompressible flows and collocated arrangements. The interpolation of the cell centered internal fields is relatively simple. The variation of the function over each control volume is assumed linear. All fields defined on cell centers can thus be mapped using the following procedure: FLOWS (1) For each point Z in the zonal mesh, find the closest point G in the global mesh.

(2) Calculate the position difference:

∆ ZG = x Z -x G .
(3.71)

(3) Calculate φ Z as:

φ Z = φ G + ∆ ZG • (∇φ) G . (3.72)
The face flux interpolation requires more care. The fluxes are defined on cell faces and satisfy the continuity constraint. If the flux transfer is not accurate, continuity will be violated, possibly causing unboundedness in the first solution of the zonal mesh and other undesirable effects.

Since not all of the zonal faces have their equivalent in the global mesh, a more general and accurate procedure is proposed in [START_REF] Jasak | Error Analysis and Estimation for the Finite Volume Method With Applications to Fluid Flows[END_REF]. For that purpose, we need to come back to the calculation of fluxes (see section 2.11.1). Fluxes are calculated using equation 3.73:

F = S •   H(U ) a P f - 1 a P f (∇p) f   , (3.73)
after the solution of the pressure equation 2.88:

f S • 1 a P f (∇p) f = f S • H(U ) a P f . ( 3.74)
Equation 3.74 guarantees that the fluxes satisfy continuity. Instead of transferring the fluxes directly, parts of the pressure equation will be interpolated to the zonal mesh. The required fields are a P and H(U ), both defined at cell centers and easy to transfer. The pressure equation is then assemble and solved on the zonal mesh before the coupled calculation is started. This procedure will always produce conservative fluxes [START_REF] Jasak | Error Analysis and Estimation for the Finite Volume Method With Applications to Fluid Flows[END_REF].

Validation of the strategy

To assess the accuracy of solutions calculated with the TPZ approach previously detailed, two 2D test cases have been set up with the proposed solver. The first configuration is a rising bubble configuration set up by Hysing et al. [2]. The second case is a turbulent jet of liquid fuel into steady ambient air. For each of these two cases, validations of the TPZ approach are based on comparisons between a simulation using a coarse global mesh coupled with a refined zonal domain and a reference simulation using a single fine mesh.

In the first test case, only RI solver is used, since it is not pertinent to use TDF solver in this laminar and separated bubble flow. The zonal grid is placed above the initial bubble position, where mesh refinement affects volume fraction gradients and bubble deformation. In that way, entrance of an isolated phase structure inside zonal grid is also investigated.

In the second test case, the zonal grid is placed in the injection zone, where mesh refinement is necessary to capture velocity gradient at the injector outlet. Three combinations of single grid solvers are applied in order to investigate influence of two phase models over results:

• RI solver in both domains.

• TDF solver in both domains.

• Hybrid: RI solver in Zonal Domain (ZD) and TDF solver in Global Domain (GD).

These model combinations are summed up later in table 3.5 along with the mesh sizes and refinements.

Rising bubble

Configuration

The rising bubble problem investigates the ascending motion of a bubble of gas inside a quiescent liquid. A benchmark of this configuration has been set up by Hysing et al. in 2009 [2] and used later for studying accuracy of interFoam solver by Klostermann et al. in 2013 [START_REF] Klostermann | Numerical simulation of a single rising bubble by vof with surface compression[END_REF].

Hysing et al. [2] distinguished two different set-ups of the numerical experiment: ellipsoidal bubble and skirted bubble. They differ by the density ratio and the viscosity ratio between both phases. We chose to reproduce the skirted set-up which is more influenced by mesh refinement: in the finest mesh, the bubble forms thin filaments with small satellite bubbles. These structure detachments do not occur when the mesh is coarse [START_REF] Klostermann | Numerical simulation of a single rising bubble by vof with surface compression[END_REF]. It is thus pertinent to apply the current zonal refinement approach on this configuration. The area of interest for refining is the liquid-gas interface. We chose to employ a single fine zone that comprise the whole bubble at t = 3s.

On the basis of the benchmark definition of Hysing et al. [2], a two-dimensional computational domain with an aspect ratio x : y = 1 : 2 is employed, see figure 3.11. The bubble is initially centered at (x, y) = (0.5, 0.5) with r b0 = 0.25 as the initial radius. The domain is fully enclosed by no-slip walls at the top and the bottom and free slip walls on the left and right sides.

The gravity vector g points towards the bottom of the domain. It is a laminar low-Reynolds case, hence without turbulent modeling. RI model will be employed to follow the interface. Primary phase α will refer to the liquid. Physical properties of the configuration are reported in table 3.2. The Reynolds number is defined as

Re = ρ 1 U g L µ 1 , ( 3.75)
with the rising velocity U g = √ g2r b0 and the bubble characteristic length L = 2r b0 .

The fine zone is placed over the initial bubble position, as shown in figure 3.11, in a region in which the highest gradients will occur during the bubble rising. In this configuration, at the interface Γ, a coupled Dirichlet condition is employed for velocity. Thus, the boundary conditions of the zonal domain consist in:

• coupled Dirichlet boundary condition for velocity U ,

• coupled inlet-outlet boundary condition for phase fraction α,

• and zero gradient condition for dynamic pressure P rgh (equation 3.62). FLOWS The zonal domain, with interface Γ, is placed above initial position, with a mesh refinement of 2 : 1.

ρ 1 ρ 2 µ 1 µ 2 g σ Re kg.m -3 kg.m -3 kg.m -1 s -1 kg m -1 s -1 m/s 2 kgs -2 -
The fine mesh refinement relative to the coarse refinement is 5 : 1 in the y-direction close to the jet center line and 2 : 1 otherwise Two different grid spacings are employed: fine and coarse. The coarse refinement consists of a Cartesian mesh with 80 and 160 cells in horizontal and vertical directions respectively. The fine mesh refinement relative to the coarse refinement is 2 : 1. Zonal simulation is performed using a global coarse mesh coupled with a fine zone. Mesh sizes with these refinements are shown in table 3.3, both for standard and zonal simulations, along with the employed two phase solver. The simulation time is t f inal = 3s with a fixed time step. The zonal sub-cycling ratio r t will be equal to grid refinement ratio r x = 2.

Results

Final bubble interface, at t = 3s, obtained with two standard simulations (coarse and fine) and the zonal simulation are reported in figure 3.12. With the coarse simulation (left), the main bubble structure is skirted and followed, by two independent small structures. By decreasing the cell size (fine case, middle in figure 3.12-(b)), two additional satellite bubbles appear. The main mushroom shaped structure shows also shorter filaments. The bubble surface obtained with the zonal simulation (right) is in good agreement with the fine one. Indeed, the two addi- Red and blue text colors respectively stand for coarse and fine mesh refinements.

t = 3s

t = 1.5s Figure 3.12: Liquid-gas interface at t = 1.5 s and t = 3 s for three simulations of Hysing skirted bubble configuration [2].

The liquid-gas interface is shown with the isocontour α = 0.5. From left to right, green line is coarse mesh, black line is fine mesh and red line is coarse mesh coupled with a fine zonal mesh. The zonal interface Γ is shown with an orange rectangular box.

tional satellite bubbles are present, with similar sizes. The two lower structures size are closer, in shape, to the coarse ones since they have not crossed the zonal interface Γ. In figure 3.12, at t = 1.5s, it can be seen that the bubble shape crosses the zonal domain smoothly without being affected by the presence of the mesh refinement discontinuity.

Quantitative results consist of the bubble rising velocity U , expressed as The vertical grey dashed line indicates the time the bubble interface is in ZD.

U = Ω α g (U • y) dΩ Ω α g dΩ , ( 3
with gas volume fraction α g = 1 -α. Evolution of this quantity is reported in figure 3.13, for the three cases. One can observe that the two velocity peak values, V max1 and V max2 , at times t = 0.7s and t = 2.0s, respectively, are higher with the fine run than the coarse one (respectively 0.63% and 2.49% higher), as well as the final velocity at time t = 3s.

Second peak V max2 decrease is more noticeable on the zoomed profile. The zonal simulation gives results that are close to the standard ones. It is in good agreement with the fine simulation until the second peak. Then, the rising velocity is governed by the two lowest gas structures.

In the zonal simulation, these structures stay outside ZD, i.e. in the coarse mesh. It explains that, after t = 2 s, the rising velocity profile obtained with the zonal simulation is closer to the coarse profile than the fine profile.

The mass conservation property of the zonal scheme has been checked. Since the computational domain is closed, the initial amount mass should remain still during the whole simulation. The maximal mass error obtained with the zonal simulation is equal to 0.005%, which is in a very low and acceptable range.

Performances

In comparison with a fully refined mesh, the zonal simulation reduce computational cost by 73%, i.e. a speedup of 3.7. This gain is higher than in the jet case due to the smaller zonal mesh size, relative to the fine mesh. During the CPU effort, the percentages dedicated to GD single grid solver, the ZD single grid solver, the prolongation step, the restriction step and the correction steps are respectively 27%, 64%, 1.5%, 0.5% and 7%. Intergrid-communications and correction step count for 9% of total CPU effort.

Liquid-air jet

Configuration

This configuration deals with turbulent injection of liquid into steady ambient air through a circular pipe. Mesh refinement inside the pipe has a major influence over jet velocity at the nozzle exit. Liquid is injected through inlet boundary with an uniform velocity of 100 m/s. Its physical properties are shown in table 3.4. Primary phase α will refer to liquid. Reynolds number at nozzle outlet Re = 10 5 demonstrates the turbulent character of the flow. Hence, a usual k -ε RANS model is used in this configuration to model the turbulence. This model solves two additional scalar fields (k and ε), which will be coupled in the zonal approach. Turbulence intensity and turbulent length scales at inlet are equal to 7.5% and 10% of the mean outlet velocity and the injection diameter respectively.

The physical boundary conditions are shown in figure 3.14 along with the grids and domain dimensions. An uniform velocity is prescribed at inlet boundary and total pressure is assigned on atmosphere boundaries. Injector walls are modeled with a no-slip condition and high-Reynolds standard wall-functions are employed for boundary layer modeling. An angular symmetry is considered and slip conditions are used along the axis.

Aforementioned, the zonal grid is placed in the injection zone, where mesh refinement affects acceleration of the fluid before the nozzle exit. Thus, two mesh refinements are studied: fine FLOWS Red and blue text colors respectively stand for coarse and fine mesh refinements.

The length of the zonal domain is set up to half of the global domain length. Its height is placed sufficiently high to avoid having high velocity gradients between the liquid jet and the steady gas in the coarse mesh. Boundary conditions of the zonal domain consists in physical (inlet, no-slip, wall and axis) and coupled (interface Γ) boundaries, as shown in figure 3.14. ALong Γ, pressure is imposed along,

Validation of the strategy 101

with values interpolated from GD. Thus, we use,

• coupled Dirichlet boundary condition for dynamic pressure P rgh ,

• coupled inlet-outlet boundary condition for velocity U , α, k and ε.

The simulations are carried out with an adjustable GD time-step, following relation 3.48. Thus, time-step ratio r t is adjusted at each time-step by applying equation 3.50. Simulations show that this time-step ratio varies in a bounded range r t ∈ [2, 5] with an average value of |r t | = 3.1.

Results (TDF model)

In this part, we discuss results obtained with the three first RANS configurations of table 3.5, i.e. using only the TDF two phase model, on both grids in the zonal case.

Volume fraction field obtained in transient state with the TDF zonal simulation is shown in figure 3.16-(a). Volume fraction and velocity fields obtained in steady state with the zonal simulation are shown in figure 3.17. One can observe the diffusion of the liquid jet under action of the turbulent diffusion flux in the TDF model. The relative velocity difference field between the zonal run and the full fine run is shown in figure 3.18-(b). It is to be compared with the field between the coarse and the fine runs in figure 3.18-(a). In field 3.18-(a), the highest differences are logically located in high gradient zones, i.e. in the transition between jet cone and steady gas, as shown in steady state velocity field in figure 3.17, and in the region close the injector wall above nozzle exit. In field 3.18-(b), the differences in these two previous zones are much lower (30% instead of 100%), especially in the jet cone region. In the corner of the zonal domain, a peak is visible. It may be explained by a difficulty of interpolation in the corner due to the first order scheme employed in the tangential interpolation of prolongation step.

Concerning quantitative results, evolution of adimensioned velocity and primary phase along the main axis are reported in figure 3 and the third quantity by a volume integral within the domain.

Figure 3.20 shows evolution of these three quantities in the zonal run. Since the injected liquid mass flux is constant, V in (t) grows linearly with time. After tU 1 /D = 30, simulation reaches a steady state and amount of liquid inside computational domain is stabilized while liquid outflow rate grows linearly. Evolutions of V in and V out + ∆V are very close with a maximum relative error of 0.35%. It shows that the relation 3.77 is satisfied using the zonal approach with TDF model in both global and zonal domains. Note that similar observations have been made in all cases presented in this work. Therefore, this point is not mentioned after.

Results (RI model)

In this part, we discuss results obtained with three RANS configurations of table 3.5, using only the RI two phase model, on both grids in the zonal case. The relative velocity differences field between the zonal run and the full fine run is shown in figure 3.22-(b). It is to be compared with the field between the coarse and the fine runs in figure 3.22-(a). In field (a), the highest differences are located in the gas region, in the transition between jet cone and steady gas and close the injector wall. In field (b), these differences are lowered, more noticeably in the zonal region. Along the grids interface Γ, some differences are also visible, highlighting weak errors induced by the zonal coupling. FLOWS V in V out V V out + V

Results (hybrid solver)

In this section, the ability of the zonal solver to handle two different two phase solvers is tested. The maximum relative mass error is less than 0.37% in this zonal hybrid configuration.

These results show that the present zonal algorithm is able to handle a hybrid approach of two-phase flows.

Performances

In comparison with a fully refined mesh, the zonal simulation reduces computational cost by 40%, i.e. a speedup of 1.7. During the CPU effort, the percentages dedicated to GD single grid solver, the ZD single grid solver, the prolongation step, the restriction step and the correction steps are respectively 15.5%, 66.0%, 9.0%, 0.5% and 9.0%. Intergrid-communications and correction step thus count for 18.5% of total CPU effort. These performances are independent of the two-phase solver employed, since RI and TDF algorithms have very close structures.

Parameter studies

In this section, several parameter studies examine the influence of the zonal method scheme variants on the results of the two previous test cases. Three aspects are particularly studied:

• Accuracy: does the scheme improves the results toward a full fine refinement solution ?

• Boundedness: does the solution stays bounded between coarse and fine solutions ?

• Mass conservation: does the scheme conserve the mass ?

The parameters which will be studied in the following are interpolation schemes (from cellcenters to face-centers, tangential interpolation, interpolation in time), coarse-fine boundary condition types, normal gradient coupling at the coarse-fine interface and the zonal domain position.

For each parameter study, we take as reference the zonal coupling scheme previously shown (see the section 3.4 about numerical coupling method) and change one parameter at a time.

F α = F × α f + F r × α f (1 -α f ) ,
can be rearranged to obtain the implicit expression (Eq. 3.55) of phase indicator at the face centers:

α f = F α F + F r (1 -α f ) .
We shall in the following refer to this interpolation scheme as the Surface Compression (SC) scheme.

(TDF) Similarly, the explicit expression for face center phase indicator field (Eq. 3.56) is derived from equations 3.28 and 3.31:

α f = ρF -F × ρ 2 -F ν,α × (ρ 1 -ρ 2 ) F × (ρ 1 -ρ 2 ) .
We shall in the following refer to this interpolation scheme as the flux derived scheme.

Let us now compare some results using either a linear interpolation scheme, either equations 3.78 and 3.78 respectively with RI and TDF models. When applying a linear interpolation scheme, the face value of α is obtained by linear interpolation between the neighbor cell centroids P and N (see figure 3.5):

α f = ωα P + (1 -ω) α N , (3.78)
where ω is the weighting factor for linear interpolation, defined as:

ω = |x f -x N | |x P -x N | . (3.79)

Application

This study is applied on the rising bubble test case, using either RI model, either TDF model.

In the liquid-air jet test case, liquid is only going out of the zonal domain. Thus, only normal gradient of phase indicator is interpolated to ZD/GD boundaries, not face values. Therefore, this parameter study has no influence over the liquid-air jet case results. (RI) Figure 3.26-(a) shows the rising velocity for coarse, fine refinements and zonal methodology with the two studied face interpolations, using RI model. Globally, zonal profile with SC interpolation is closer to the fine profile than the zonal one with linear interpolation. The first maximum velocity V max1 obtained with SC interpolation is close to the fine value (-0.15%) and greater than the coarse value, while the one obtained with a linear interpolation gives a value lower than the fine (-1.11%) and coarse values. Then, the tendency to decrease is better captured with the SC interpolation than the linear interpolation.

(TDF) Figure 3.26-(b) shows rising velocity for coarse, fine refinements and zonal methodology with the two studied face interpolations, using TDF model. Globally, zonal profile with flux interpolation is closer to the fine profile than the zonal one with linear interpolation. The gain is less pronounced than previously, when using RI model and SC interpolation. This is due to the fact that here, the liquid-gas interface is diffused. Thus, the phase indicator gradient is less steep and a linear interpolation provides correct results. Both zonal profiles are out of coarse and fine bounds.

Mass conservation

(RI) Evolution of relative mass error is reported in figure 3.27-(a) obtained with coarse, fine and zonal simulations. Fine and coarse profiles, as shown in previous part, are fully mass conservative. Zonal profile obtained with SC interpolation highly decreases mass error compared to the one obtained with a linear interpolation. Maximum mass error magnitude is approximatively 0.005% with surface compression while it is 0.1% with linear interpolation. (TDF) Evolution of mass error is reported in figure 3.27-(b). Same tendency is observed: using flux derived scheme preserves better mass than a standard linear scheme. Maximum mass error magnitudes are 0.0015% and 0.015% respectively with flux and linear interpolations. This last one shows a smaller error when using TDF model than when using RI model, since liquid-gas interface is diffused.

These two results highlight the importance of the face interpolation methods regarding the conservative aspects of the coupled solver presented here. The surface compression and flux interpolation schemes should be used for zonal simulations using respectively RI and TDF models in the global domain.

Time interpolation schemes influence

Schemes

Here we investigate the influence of the time interpolation scheme in the prolongation step of zonal algorithm (step (2.1), see figure 3.8). This parameter study is applied on the bubble rising test case. The considered fields are all variables interpolated during step (2.1), i.e. velocity U , phase indicator α and its normal gradient ∇ ⊥ α.

Let's consider an arbitrary field variable φ, that can be a scalar or a vector, in Global Domain (GD). After resolving GD over a time-step ∆t, solutions for φ are known at instants t n (beginning of GD time-step) and t n+1 (end of GD time-step), with respectively φ(t) and φ(t + ∆t). We aim now to obtain boundary conditions for Zonal Domain at GD/ZD interface Γ. As a reminder, Zonal Domain is refined in time, thus, ZD time-steps are sub-cycled. The time-step ratio between GD time-step (∆t)and ZD time-step (∆τ ) is r t = ∆t ∆τ . Thus, the boundary conditions of ZD are defined at the time t + k∆τ , where k ∈ [1, r t ] is the current sub-cycling iteration. Hence, interpolation in time is necessary to obtain boundary values at the interface Γ. two Taylor series, at instants t + ∆t and t + k∆τ :

φ(t + ∆t) = φ(t) + ∆t ∂φ ∂t t + O 2 , ( 3.80)
φ(t + k∆τ ) = φ(t) + k∆τ ∂φ ∂t t + O 2 . (3.81)
The three schemes are presented below.

φ(t + k∆τ ) = φ(t) + k r t (φ(t + ∆t) -φ(t)) + O 1 . (3.86)

Application

The three previous schemes are tested on the rising bubble problem, using RI model. The mesh and time refinements between ZD and GD equal to 2: r t = r x = 2. The base coarse and fine meshes own respectively 80 cells and 160 cells in x-direction.

Rising velocity evolutions are reported in figure 3.28 for the three zonal runs and the two uniform mesh runs. It can be first observed that explicit injection is not bounded at all by coarse and fine profiles. Location of inflections of velocity are approximatively at same instants (0.5s and 2.1s) but values are far below coarse mesh values. Second observation concerns the two other schemes, implicit injection and linear interpolation. Both schemes provide good results that are in close agreement with coarse and fine mesh profiles. In zoomed figure (b), between instants 1.0s and 1.5s can be observed, the linear scheme profile is closer to the fine and coarse mesh profiles than the implicit one.

As a conclusion about the time interpolation schemes, the first order linear interpolation in time scheme should be used for zonal simulations with time sub-cycling.

Tangential interpolation schemes influence

Here we investigate the influence of tangential interpolation scheme in the prolongation step of zonal algorithm (step (2.1), see figure 3.8). Tangential interpolation means interpolation between two coincident faces, with one fine face overlying a coarse one. As shown in figure 3.9, the considered fine face centered is indexed by i and located at the zonal interface Γ. The nearest coarse face center is indexed by I and enclosed by the coarse faces I -1 and I + 1.

Schemes

Three tangential interpolation schemes are studied [START_REF] Manhart | A zonal grid algorithm for {DNS} of turbulent boundary layers[END_REF]:

• Injection: prolongation by injection is a 1 st order method. It is also referred to as the "nearest value" method. It supposes that the variable is constant in space:

φ i = φ i+1 + O 1 , ( 3

.87) FLOWS

with i and i+1 the indexes of two neighbor faces in ZD. This approximation is conservative in mass but not in momentum. A face centered variable φ f , at i, is thus equal to φ f at I:

(φ f ) i = (φ f ) I . (3.88)
• Linear interpolation: This interpolation scheme is 2 nd order accurate. It is expressed as a function of φ on coarse faces indexed by I and I -1(see figure 3.9):

(φ f ) i = (1 -ω) (φ f ) I + ω (φ f ) I-1 , (3.89)
where ω is a weight function, expressed as:

ω = x I,i • x I,I-1 x I,I-1 • x I,I-1 , ( 3.90)
with x I,i = x I -x i the distance between face centers I and i. This interpolation technique is not mass conservative [START_REF] Manhart | A zonal grid algorithm for {DNS} of turbulent boundary layers[END_REF].

• Left and right-skewed linear interpolation: This interpolation scheme blends a left-skewed and a right-skewed linear interpolation, and is 2 nd order accurate [START_REF] Manhart | A zonal grid algorithm for {DNS} of turbulent boundary layers[END_REF]. It is expressed as a function of φ on coarse faces indexed by I,I + 1 and I -1 (see figure 3.9):

(φ f ) i = (φ f ) I + ω I+1 (φ f ) I+1 + ω I-1 (φ f ) I-1 , (3.91)
with ω I+1 a weight function for φ value at face I + 1, expressed as

ω I+1 = x I,i • x I,I+1 x I,I+1 • x I,I+1 , (3.92)
and ω I-1 a weight function for φ value at face I -1, expressed as

ω I-1 = x I,i • x I,I-1 x I,I-1 • x I,I-1 . (3.93)
This interpolation technique is mass conservative [START_REF] Manhart | A zonal grid algorithm for {DNS} of turbulent boundary layers[END_REF].

Application

These three schemes are applied on the rising bubble problem, using RI model. It is tested in zonal simulations with refinement in time and space equal to 2: r t = r x = 2. The base coarse and fine meshes own respectively 80 cells and 160 cells in x-direction. The considered fields are all variables interpolated during step (2.1), i.e. velocity U , phase indicator α and its normal gradient ∇ ⊥ α .

Rising velocity evolutions are reported in figure 3.29. Let us look at the first velocity peak V max1 . The skewed linear interpolation peak is the closest to the fine value. Then comes injection peak and at last the linear peak. The skewed interpolation V max1 value is bounded by coarse and fine values, at the opposite of the other schemes. Linear profile, which is second Scale is zoomed on velocity maximums. order accurate, shows lower peak than the first order injection scheme. This is due to the lack of mass conservation in this linear scheme. Same parameter study is applied on the liquid-air jet configuration. The considered fields are all variables interpolated during step (2.1), i.e. velocity U , its normal gradient velocity ∇ ⊥ U , phase indicator α, its normal gradient ∇ ⊥ α, dynamic pressure P rgh and turbulent scalars (k and ε).

It provides a different conclusion. Since information is mainly leaving the domain, interpolation scheme and its order of accuracy have here a null influence on quantitative results, as shown in FLOWS As a conclusion for r x = 2, injection and skewed linear interpolation schemes provide correct results thanks to their mass conservative aspect while linear interpolation scheme should be avoided since this second order scheme provides worse results than the first order scheme, due to a lack of mass conservation.

Note: For the parallelized version of the solver, in order to ease the implementation, only injection space interpolation is available.

Neumann condition in coupled inlet-outlet boundary conditions

As described in the proposed zonal methodology section, one applies at the coarse-fine interface a coupled inlet-outlet boundary conditions for velocity and other scalar quantities (depending on the configuration).

A coupled inlet-outlet boundary condition consists to impose an interpolated field quantity from GD if volumetric flux is going in ZD and to impose a normal gradient if volumetric flux is going out from ZD. Two possibilities arise concerning this normal gradient:

• Either use information from GD and interpolate the coarse surface normal gradient onto ZD interface (apply P(∇ ⊥ φ) ).

• Either use a simple zero gradient condition (apply ∇ ⊥ φ = 0).

The second possibility is simple to implement and first order accurate. It is similar to an upwind scheme. The first possibility is of higher order of accuracy, however, it can leads to unboundedness of the solution, as shown later. We investigate there after the influence of gradient coupling on the results accuracy, boundedness and mass conservation in the two previous test cases.

Accuracy and boundedness of velocity

In rising bubble test case, figure 3.32 shows rising velocity profiles using either zero gradient, either coupled gradient. Coupling the gradient does not impact the magnitude of the first peak but it does improve the following tendency to decrease, that is in better agreement with fine profile than using zero gradient.

Mass conservation and boundedness of phase fraction

Normal gradient interpolation has an impact on boundedness of volume fraction field in ZD, FLOWS thus on mass conservation. In the liquid -air jet configuration, α values close to the interface are not bounded and need to be clipped . A clipping process consists to impose a one value when it is greater than one and a null value when it is lower than zero. Figure 3.33 shows the cumulative amount of liquid volume fraction that is clipped in ZD during the resolution of the liquid-air jet case, when using respectively (a) RI and (b) TDF model. The cumulative amount of liquid clipped is divided by the cumulative amount of liquid volume fraction that is going inside GD since the beginning of the simulation.

Concerning RI model, clipping is necessary and performed when normal gradient is coupled. It starts around tU/D = 13, i.e. when liquid jet is crossing the coarse-fine interface Γ. At this moment, the amount clipped is negative, meaning that phase fraction values have been below 0 and it has been necessary to "add" liquid in those cells. Then, the amount clipped at each time step is positive and is decreasing asymptoticly toward zero with the simulation reaching steady state. The cumulative amount that has been clipped is less than 0.5%, which is in a reasonable range. When zero gradient is used, none clipping is necessary, boundedness in ZD is respected.

Concerning TDF model, coupling the gradient does not have an impact on boundedness since using coupled gradient or zero gradient show the same results. The absolute cumulative amount is here much lower with TDF model than RI model, i.e. 1 × 10 -5 % instead of 0.5%, showing that the diffuse model allows a better conservation at the coarse-fine interface Γ. Figure 3.34 shows the relative mass error in the rising bubble test case. The relative mass error is the relative difference between the initial mass and the mass at time t. The global domain is closed. Zero gradient scheme shows a fully conservative simulation, with a null error from the first to the last instant. Coupled gradient shows an increasing error starting at the moment the bubble enters in ZD that reaches the very weak relative value of -3.5 × 10 -3 %. As a conclusion about this parameter study, coupling the normal gradient in the prolongation step improves the accuracy of the results. On the other hand, it deteriorates in a very low and reasonable range the mass conservation, due to the interpolation process. Thus, we chose to focus on accuracy and shall use this parameter in the later simulations. Zonal Domain interface at x = 11D is indicated by a vertical dashed line.

Influence of velocity and pressure boundary condition types at the interface

The coupled boundary conditions are located at the coarse-fine interface Γ. Informations from the underlying global mesh are interpolated to this interface. Let us interest on the velocitypressure coupling. One first and natural possibility, denominated approach (a) consists to impose fluxes at the zonal boundary by interpolating velocity from GD. This approach has the shortcoming that the zonal velocity field is over-constrained and accuracy of the fine mesh is diminished. An alternative, denominated approach (b), consists to let the accurate information of ZD velocity to leave the domain with a Neumann condition and to impose flux from GD when information is going in. As a consequence, due to the incompressible velocity-pressure coupling, Neumann condition for pressure is imposed in approach (a) and a Dirichlet condition is imposed in approach (b). In the later, since pressure is known in GD, it is interpolated to ZD interface. A limitation of approach (b) is when RI model is used in ZD: Imposing pressure at the coarse-fine boundary Γ mays cause unphysical effects on the flow because of the pressure jump at the liquid-gas interface, such as suction force. Nevertheless, these unphysical effects have not been spotted in the current two test cases, as shown later.

To summarize, two possibilities arise for setting velocity and pressure boundary conditions at ZD interface Γ: In this section, we study the influence on accuracy and boundedness of the results of using one of these two conditions. FLOWS The profile obtained with such configuration is in better agreement with fine results than the combination (a): the rising velocity is not impacted by the upper interface in the last moments of the simulation (tU/D = [2.6, 3]).

As a conclusion, the inlet-outlet condition for velocity allows more degrees of freedom to a flow leaving ZD and is more adapted for simulating a atomization test case. The zonal domain should own at least one Neumann boundary condition for pressure, either at physical boundary condition (inlet,wall), either at the coupled interface Γ. However, there is room to improve the numerical coupling: a volumetric flux correction step should be performed after the restriction step in order to correct velocity in coarse cells along the coarse-fine interface Γ. This inlet-outlet condition is also used for the other scalars such as phase indicator α and turbulent scalars (k, ε,...).

Zonal domain position influence

As stated by [START_REF] Joel | Computational methods for fluid dynamics[END_REF] when referring to overlapping grids, the interpolation process may introduce errors or convergence problems if the solution exhibits strong variations near the interface. In our work, ZD/GD interface are coincident, this reduces errors coming from the prolongation step. However, the point which is highlighted is that the coarse-fine interface should be placed in zones with weak flow variations. This is the point that is studied here, by modifying size and position of the zonal domain in the two test cases.

Concerning liquid-air jet test case, three ZD lengths are studied: 5.5D (short),11D (medium and 16.5D (long), that correspond respectively to 1/4, 2/4 and 3/4 of GD length, excluding inlet pipe. Scale is zoomed on velocity maximums.

atmospheric GD right boundary with medium size ZD and is increased with large size ZD. It shows that the ZD/GD interface should be placed sufficiently far from GD boundaries.

Concerning rising bubble test case, three positions and sizes are studied: high (original position, above initial bubble position), low (around initial bubble position) and tall (from lower interface in low position to higher interface in high position). The zonal domain tall configuration covers the whole displacement of the bubble, thus liquid gas interface does not cross the coarse-fine interface Γ. These positions are shown in figure 3.39. Figure 3.40 shows rising velocity profiles. The tall configuration provides the best results for both interpolation schemes. The curves are quasi fully bounded from 0.5s to 2.5s. Then, when bubble and volume fraction gradients are closer to the upper coarse-fine interface, both profiles diverge above fine '1/h = 160' profile because of the coupled Dirichlet condition for velocity. In the 'low' profile, this behavior is absent because ZD is placed lower.

As a conclusion, the position of the zonal interface Γ matters: it should be placed far enough from the global domain (GD) boundaries, as seen in the liquid-air jet results, and from the GD zones in which the highest gradients will occur during the simulation. In the liquid-air jet case, the correction of ZD persists downstream the zonal interface Γ on a few diameters.

Influence of corrections on solution

In this section, influences of the two active corrections performed after the restriction step (step (4) in zonal algorithm) are investigated. These corrections account for the correction of the liquid volume fraction in coarse cells along coarse-fine interface Γ and for the divergence-free correction of the face flux field in GD. FLOWS Zero gradient is used instead of coupled normal gradient for α inlet-outlet boundary condition in ZD.

Liquid volume fraction correction influence

At the coarse-fine interface Γ, fine and coarse volume fraction fluxes are mismatched. The cell-centered restriction step will correct the α values in the covered part of GD, but not in the cells along ZD interface, that depend of the interface fluxes. Thus, as detailed previously, equation 3.70 is applied over all cells along the zonal grid interface Γ:

α n+1 corr = α n+1 - ∆t V R f (F α,o ) Γ -(F α,o ) Γ .
Let's show the influence of the correction on the rising bubble test case, that is more sensitive to this mass conservation issue than the liquid-air jet case, since an individual particle crosses the coarse-fine interface Γ. Two simulations are runs, with and without this volume fraction correction procedure. The normal gradient coupling, at the boundary condition of α, is also turned off in order to improve mass conservation in these two simulations: a zero gradient condition is used instead.

Figure 3.41 shows the relative mass error evolution with these two runs. The maximum value is -0.05% without this correction, due to the loss of mass through ZD boundaries. With the correction, maximum error is very low (-6 × 10 -6 %). It is close to the fine simulation error value (-3 × 10 -7 %).

A similar comparison will be performed later on a more complex configuration, in which the maximum relative error is relatively high without this correction.

Divergence free correction influence

After the restriction step, flow in cells along coarse-fine interface Γ is not divergence free, i.e. divergence of the velocity is not null:

∇ • U = 1 V f F = 0 . (3.94)
In the restriction step, face-centered volumetric fluxes F , that are divergence free in zonal domain, are interpolated to the underlying faces in global domain (see figure 3.10-(c)). Because of the flux mismatch, discontinuity occurs along Γ. To ensure a divergence free flux field in the whole global field, a Poisson equation is solved to correct the face flux field. We aim here to measure in which order this correction affects solution.

In rising bubble configuration, coupled boundary conditions in ZD are fully Dirichlet for velocity. Thus, the face fluxes are imposed all along the interface Γ and can not be adjusted during the resolution of the ZD solution. In other words, the boundary face fluxes and the underlying coarse face fluxes are strictly equal. As a consequence, for a full Dirichlet coupled boundary conditions in velocity, the flux mismatch does not occur and the following statement is true:

F GD Γ = R f F GD Γ . ( 3.95)
A face flux correction step to ensure a divergence-free face flux field is unnecessary in this configuration.

On the other hand, in the jet configuration, coupled boundary conditions in ZD are inlet-outlet for velocity, i.e. Dirichlet when flux is going in ZD, Neumann when flux is going out from ZD.

The flux mismatch occurs and the statement 3.95 is not true. A correction is thus necessary in this configuration.

To visualize variation of face fluxes in the software Paraview R , that allows to show only cell center fields, it is necessary to post-process the face flux field F . We introduce a cell center reconstructed velocity U rec , defined as:

U rec =   f (n ⊗ S)   -1 •   f (nF )   . (3.96)
In OpenFOAM R library code formalism, previous equation is written as:

U_rec = fvc::reconstruct(phi)
To measure influence of the face flux correction procedure, we monitor relative variation of this cell center reconstructed velocity. Its relative variation is defined as: It can be first observed that the maximum amplitude of this difference is 4%, except at two singular points where amplitude reaches 4.7% at tU/D = 15 and 8% at tU/D = 25. Second, it can be observed that this relative difference is close to zero in majority of the Zonal Domain part. This is due to the boundary condition of the correction pressure p corr , that are equal to those of the dynamic pressure P rgh . Indeed, it is zero gradient condition for inlet and FLOWS walls, and fixed value for the atmospheric boundaries. Thus, face fluxes can not be corrected along inlet and walls while it can be along atmospheric boundaries . Third and last observation, some differences are visible close to the interface Γ. The maximum values are located in the top-right corner, after tU/D = 25. These observations show that the face flux correction modifies face flux amplitudes in a reasonable range, i.e. less than 10% , and that these modifications are mainly located outside the Zonal Domain region.

= |U rec | |U old rec | -1 , ( 3
To go further in the analysis, two simulations are performed with and without this divergence free correction step. Note that the liquid-air jet is a sufficiently simple test case to be able to converge despite this correction procedure. Figure 3.43 show relative velocity differences between the fine simulation and these two zonal simulations. In both fields show the highest error near the right atmospheric boundary. This error spot has been seen previously in figures 3.38-(c) and 3.38-(d) respectively with the medium and long zonal domain sizes. This error is explained by the interface Γ being too close to the GD atmospheric boundary.

The lower field shows that without the correction, differences are higher along the top coarsefine interface Γ than with in the upper field with the correction. Indeed, this differences are located in cells with important divergence free error. As well, differences are weakly higher in some parts above zonal domain with correction than without (3% instead of 1%). Figure 3.44 shows velocity profile along jet center line when steady state is reached, for the two zonal simulations, with and without correction. Differences between the two profiles are hardly noticeable.

As a conclusion, this divergence free correction allows to obtain a divergence free face flux field in GD at the end of a time-step, by correcting the fluxes mainly outside the ZD part. The numerical solution is very weakly affected. First one (on top) is the relative difference between fine and zonal method with divergence free correction. Second one (on bottom) is between fine and zonal method without this correction.

Introduction

Parallel computing is defined as the simultaneous use of more than one processor to run a program. For a given fixed problem size, it consists to divide it in smaller pieces. Each piece owns its own set of data and its own processor. All these smaller tasks will be then executed at the same time. The main purpose is to obtain the solution of the problem in a reduced time lapse. It requires though regular transfer of informations between processors and thus adaptation of the program to parallel computing.

In CFD, the given fixed problem is a discretized domain, with a certain amount of elements. Parallel CFD consists to decompose it into smaller domains and solve the governing equations on each of these sub-domains. Each one will share common boundaries with its neighbor subdomains. This is done with one Domain Decomposition Methods, as it was described previously in the literature review part of this chapter. Special attention has to be made concerning load balancing: the number of elements should be equitably distributed between the processor, in order to optimize the use of resources and to avoid overload of any single processor.

In OpenFOAM R , patched grids method is used to decompose the domain: a processor subdomain shares a simple patch with its neighbors. Figure 3.3-(a) shows this type of grid layout. Internal boundaries between the different parts of the mesh are called processor patch in the software library. Division of the domain can be done automatically using the scotch decomposition method. This method attempts to minimize the number of processor boundaries, i.e. the required amount of data to share between processors. It thus improves the performance of the parallel run.

It can also be done with a simple decomposition method in which the domain is split into pieces by direction.

In the two previous methods, load balancing is automatically handled.

Inter-processor communication is achieved through sending messages using Message Passing Interface (MPI) library, one of the most popular protocol used to exchange messages from one memory location to another. The parallel communications in OpenFOAM R are implemented in the linear algebra functionality and discretization methods of the tool library. A given matrix is divided into smaller matrices and solved iteratively (if implicit) with exchange of boundary data at each processor boundary at each iteration. For an explicit solving, exchange of boundary data if performed once at the beginning of the process. Thus, any solver already implemented in OpenFOAM R library (or set up by the user by changing the governing equations) is parallelized and adapted for parallel computing.

The zonal methodology described in this thesis has been implemented in the OpenFOAM R software. It has been previously validated on two simple two-dimensional test cases, using one processor. Now, in order to run it on more complex configurations with a greater number of elements, such as a primary atomization application case, we aims to use it in parallel. Both axis are log scaled.

Processor arrangements

The particularity of the zonal solver is that it couples together two single-grid solvers, already parallelized in OpenFOAM R library: interFoam (RI model) and twoLiquidMixingFoam (TDF model). Each solver owns its own set of data and mesh. Each mesh can be divided using one of the method previously described, simple and scotch decomposition methods. One can also use a manual decomposition in which the user specify the delimited region for each processor. Concerning processor arrangement in both meshes, three possibilities arise, that are illustrated in figure 3.45:

• (a) Unified decomposition: Divide one of the two domains, either GD, either ZD, using one of the OpenFOAM R splitting methods. The other domain is cut following the same borders defined in the first domain. With this decomposition, the first domain to be split is load balanced while the other one is not. The only advantage to use this structuring is that it avoids parallelization of intergrid communications. Indeed, intergrid neighbors are located on the same processor, transfers of data during prolongation and restriction steps are thus local, it does not need MPI communications. On the other hand, two drawbacks arise. The first one and the more important is that one domain is not properly parallelized: the number of divisions and the load balancing are clearly not optimized. Consider the worst case in which GD is very large compared to ZD. GD is split first, with proper load balanced, then ZD is cut following same borders. In that case, ZD could own only one processor, if there one single processor underlying region in GD. The second drawback is that it limits tangential interpolation schemes in prolongation step to first order, for faces close to a processor patch. Thus, this structuring is not considered in this thesis.

• (b) Equivalent decompositions: Each domain is split following OpenFOAM R DDM methods ( simple or scotch methods) independently one from the other and the number of processors is identical in each domain. Main advantage of this method is that each domain is load balanced. On the other hand, since both domains use the same FLOWS number of CPU cores, the smallest domain, number of elements speaking, may be not optimized for a parallel simulation.

Indeed, as shown in figure 3.46, CPU time usually decreases when the number of CPU cores increases, until one inflection point where CPU time is increasing, because parallel communications cost more than the solving itself. In computational dynamics, this case happen when the number of elements per processor is very low, e.g. less than 1000.

Thus, this type of inflection point could occur for the smallest mesh in a zonal simulation. For instance, in one configuration of the latter application presented in chapter 5, ZD fine mesh counts 5.5M of elements while GD coarse mesh counts 260k elements. Let's say a parallel simulation is performed using 480 processors. The number of elements per processor in ZD and GD is 11.5k and 540 respectively. In that case, interprocessor communications in GD will certainly cost more than solving GD equation system itself. As a consequence, the CPU efforts to solve GD with 540 processors may be more important than with twice less processor.

Nevertheless, this drawback has to be balanced by the CPU cost relative to each domain, GD and ZD. The parallel inefficiency concerning the smallest domain is compensated by its relative small size, thus small CPU cost, compared to the other domain.

As a conclusion, this processor arrangement (b) can have some limitations if the number of elements in one domain is far greater than the other one but these limitations are balanced by the relative small cost of the smaller domain.

• (c) Optimized decompositions: Each domain is split following OpenFOAM R DDM methods ( simple or scotch methods) independently one from the other and the number of processors can be different in each domain. This configuration allows each domain to be load balanced and optimized in terms of number of processors. However, one limitation of OpenFOAM R is that each mesh must be run with the same number of processors. Thus, this arrangement is currently not realizable.

The chosen configuration in this work is the configuration (b).

Parts of the algorithm to be parallelized

Following the processor arrangement (b) (equivalent decompositions), the parts of the algorithm that need to be parallelized are the communications between the domains (GD and and ZD), i.e. the restriction and prolongation steps. Figure 3.47 shows these two parts in the zonal solver algorithm, with orange dashed rectangles around.

There is only one type of prolongation process in our zonal algorithm: face-centered prolongation process involving transfer of informations between an internal face in GD and a patch face in ZD. In case of a parallel simulation, this process might also involve a processor patch face in GD, depending on the sub-domains parallel decomposition. There are two types of restriction processes: cell-centered restriction from internal field in ZD to internal field in GD, and face-centered restriction from internal field in ZD to internal field in GD. In case of a parallel simulation, face-centered restriction involves also processor patch faces, both in ZD and GD. These three types of interpolations are illustrated in figure 3.10 and need to be parallelized.

The idea of the parallelization performed here is to develop a structure that works both for serial and parallel runs. Donors, that are elements furnishing information, and acceptors, that are elements receiving informations, will be associated using data lists stored in memory. The base class for the association of two domain entities is the donors/acceptor pair. It associates one acceptor with one or severals donors.

The parallelized algorithm described in appendix A is derived from the one used by overset mesh solvers in Foam-extend version 4.0, released in January 2017 [118]. Overset mesh method is another nomination of the Chimera method, an overlapping methodology detailed in DDM section 3.2.2. This algorithm is close to our seeking, but shows the following differences:

• Overset mesh algorithm is based on a single mesh. Thus, interpolations are proceeded FLOWS between different mesh regions. In our solver, interpolations are performed between two different meshes.

• Exchanges are achieved between one donor cell and one acceptor cell. Possibly, extended donors can be added, that are the nearest neighbor cells of the donor cells. In our solver, we seek to achieve exchanges between all fine cells overlying one acceptor cell, for the cellcentered restriction process. Furthermore, faces are also involved, whether from coarse to fine in the prolongation step, whether from fine to coarse in the face-centered restriction step.

• Mesh regions are allow to move relatively to each other. Donors/acceptors Connections are thus updated at each time-step. In our solver, mesh motion is not considered. As a consequence, donors/acceptors connections can be established only once at the beginning of the simulation.

The description of the donors/acceptors associations algorithms for the three types of interpolation is given in appendix A.

Parallelism validation

Validation of previous parallelization developments has been performed on the two dimensional rising bubble test case. The same configuration than the one described previously in part 3.5.1 is used: the refinement ratio between global and zonal meshes r x is set to 2 and the ZD mesh is placed above initial bubble position; RI model is used in both domains. The same interpolation schemes and parameters are used at the exception of the tangential interpolation scheme that is a first order injection scheme (Eq. 3.88) along the whole interface Γ.

We use the OpenFOAM R simple method to split each domain respectively in 4, 12 and 64 subdomains. One serial and three parallel simulations with previous decompositions are performed until t = 3s of physical time.

Liquid-gas interface at t = 3s is shown in figure 3.48. All interface contours are quasi-identical, i.e. some very weak differences can hardly been observed. Rising velocity profiles are shown in figure 3.48. Differences between the curves can not be observed.

These qualitative and quantitative results validate the parallelization of the proposed zonal algorithm using processor arrangement (b) (see figure 3.45) and the simple domain decomposition method.

It is to note that, in these three parallel runs, the following particular case was avoided on purpose: Some processor patch faces in GD are coincident with the ZD interface Γ. This particular case has not been taken in account in current parallelization developments of prolongation process. Thus, scotch method for dividing ZD and GD domains should be avoided because it may easily lead to this particular case.

Parallel performances of the zonal algorithm will be studied in the next application chapter, on a three dimensional atomization configuration. The liquid-gas interface is shown with the isocontour α = 0.5. Black, green, blue and red lines correspond respectively to 1, 4 12 and 64 processors. Since interfaces are quasi-identical, only red line is visible.

Summary and discussion

In this chapter, an algorithm that allows for multi-scale and multi-approach resolution of turbulent and laminar two-phase flow within the Finite-Volume framework OpenFOAM R , has been presented. One advantage of the algorithm lies in sub-cycling in time that allows to refine grid locally without impacting the global computational time-step. Another advantage is the possibility to use two different single grid two-phase solvers, a sharp interface solver in one part of the computational domain and a diffuse interface solver in the rest of the domain.

Qualitative and quantitative measures have been used to validate the zonal approach. Simulation of a rising air bubble, based on the benchmark of Hysing et al. [2] has been carried out, with a refined zone placed above initial bubble position. It shows good agreement with the fully refined solution, the bubble crossing the coarse-fine interface smoothly. RANS of a two-phase circular jet has been also carried out with grid refinement in the first half of the domain. Zonal solutions show good agreements with fully refined mesh, with both sharp and diffuse interface models. An hybrid model has been applied successfully, with sharp FLOWS interface in the refined zone and diffuse in the rest of the domain. Mass conservation has been checked; the zonal coupling respects this conservative aspect inherent to finite volume solvers. In both test cases, the benefit of the zonal approach in term of computational cost is obvious in that the computational time is reduced.

This study demonstrates that the present two-phase zonal approach can be successfully applied in perspective to atomization simulation with satisfactory performance: the sharp interface model will be employed near the injector in the primary atomization region while the diffuse model will be used in the dispersed spray area.

Parallelization of the inter-grid communications has also been performed, in order to apply this coupled solver on more complex configurations. The parallelization developments have been validated on the bubble rising test case, in a range of processors between 1 and 64.

Chapter 4

Coupling SPH with finite volume

Introduction

In the scope of meshless particle methods, numerical method Smoothed Particle Hydrodynamics (SPH) is capable of treating highly convective problems with liquid-gas interfaces.

It is therefore a suitable candidate for solving primary and secondary atomization, processes in which convection is predominant over diffusion. SPH simulations of airblast atomizers performed in Karlsruhe Institue of Technology (KIT) are a good demonstration [START_REF] Braun | Modeling fuel injection in gas turbines using the meshless smoothed particle hydrodynamics method[END_REF][START_REF] Braun | Hpc predictions of primary atomization with sph: Challenges and lessons learned[END_REF][START_REF] Koch | Prediction of primary atomization using smoothed particle hydrodynamics[END_REF].

Further in the spray, the length scale of the dynamic field increases but the scale of the spray decreases or at least remains very small. A sufficiently number of particles should thus describe the smallest liquid structures, even far away from the injector. This the same issue than with Interface Capturing Method (ICM) as Volume Of Fluid (VOF). A solution could consist to increase the number of particles using an Adaptive Particle Refinement (the equivalent of Adaptive Mesh Refinement for SPH) method [START_REF] Chiron | Couplage et améliorations de la méthode SPH pour traiter des écoulements à multi-échelles temporelles et spatiales[END_REF]. However, in the dispersed spray region, diffusion becomes predominant over convection. Eulerian methods are more likely able to describe accurately these type of diffusive flows than a Lagrangian method. Therefore, another solution consists to switch to Eulerian method, as a sub-grid spray model, in the rest of the domain.

In previous chapter, a zonal methodology was presented and validated. This method consists to couple together a zonal domain and a global domain in which two different numerical methods are solved. Validations were performed by using finite volume based-methods in both domains. In this chapter, we aim to use SPH instead of the FV method in the zonal domain.

The outline of this chapter is as following. First, the numerical method SPH will be presented. Second, investigations of the potential of the SPH method are performed with an in-house code. Third, a short review about works coupling SPH with the FV method will be given. Fourth, the strategy and interpolation employed in the coupling will be detailed. Fifth and finally, extension of the zonal method for coupling SPH with Finite Volume will be applied on a laminar and single phase flow configuration.

Smoothed Particle Hydrodynamics

Historically, Smoothed Particle Hydrodynamics (SPH) was first introduced to solve astrophysical problems in three-dimensional open space by Lucy [START_REF] Leon | A numerical approach to the testing of the fission hypothesis[END_REF] and Gingold & Monaghan [START_REF] Robert | Smoothed particle hydrodynamics: theory and application to non-spherical stars[END_REF]. Since the method has been modified and adapted to solid dynamics [START_REF] Ld Libersky | High strain lagrangian hydrodynamics -a three-dimensional sph code for dynamic material response[END_REF] [124], fluid dynamics [START_REF] Joe | Smoothed particle hydrodynamics[END_REF] and explosions problems [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF]. SPH method may be synthesized in three points:

(1) It is a Lagrangian method, meaning that governing equations are solved in Lagrangian forms (see chap. 4.2.1). The equations are solved by considering control volumes or particles which are free to move in space . Hence, a motion equation is necessary.

(2) It is a meshless method, meaning that there is no topology that links different particles between them. They are independent from each others.

(3) It is based on an integral approximation method for evaluating fields associated to particles. The integral approximation is a sort of interpolation, so-called smoothing interpolation, which has been already used in Vortex method [START_REF] Cottet | Vortex methods: theory and practice[END_REF] for remeshing or in data treatments [START_REF] Isaac | Contributions to the problem of approximation of equidistant data by analytic functions[END_REF].

This method has several advantages, for instance:

• It is well adapted for multi-phase problems, since each particle can be assigned to a phase. It is also appropriated for simulating hydrodynamic fluid flows, where the density ratio between the two fluids (air and water) is high (>500). Gas phase may hence be neglected, allowing to save great computational resources since only one phase is modeled.

• Advection is treated explicitly, since particles carry their properties with them.

• It easily handles complex geometries and interactions with moving or deformable bodies since its meshless nature permits to avoid time-consuming re-meshing at each time step.

Disadvantages of the method include mostly accuracy and stability concerns, because of the use of explicit schemes for temporal discretization. Also, due to its weakly compressible treatment, its computational cost is higher than incompressible methods. High velocity gradients are difficult to handle, generating particle deficiencies. Finally, inlet/outlet boundary conditions is still an issue nowadays with difficulties to insert particles inside computational domains.

Lagrangian and Eulerian forms

There are two fundamental frames for describing the physical governing equations: the Eulerian description and the Lagrangian description. The Eulerian description is a spatial description. The discretization method is spatially fixed and the points or control volumes which are associated to are independent from the physical system which is numerically solved.

The Lagrangian description is a material description. The elements, control volumes or particles are not spatially fixed and evolve with the physical system. These two descriptions are represented in figure 4.1. For example, mass conservation equation, for incompressible flow, can be described below in these two forms:

SPH integral interpolation 4.2.2.1 Integral representation of a function

Let's consider a sufficiently smooth scalar or vector field f (x) in the domain Ω. Derivation of SPH representation starts from following identity [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF],

f (x) = Ω f (x )δ(x -x ) dx , (4.4)
where the Dirac delta function δ(x -x ) is defined as,

δ(x -x ) = 1 x = x , 0 x = x . (4.5)
Thus, it verifies the following condition,

Ω δ(x -x ) dx = 1 . (4.6)
The main concept of the SPH method is to "smooth" the delta function. Therefore, Dirac term δ(x -x ) is replaced by a smoothing kernel function W (xx , h):

< f (x) >= Ω f (x )W (x -x , h) dx . (4.7)
Kernel function W depends on the smoothing length h and the distance between positions x and x . It is homogeneous to the inverse of a distance, area or volume, depending on number of dimensions in the considered problem (1, 2 or 3). More details are given about the smoothing function in section 4.2.3.

Order of accuracy of the kernel approximation of a function

The kernel approximation is second order accurate, as long as two conditions are fulfilled. Demonstration is detailed there after [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF]:

Errors in the SPH integral representation can be roughly estimated using the Taylor series expansion of f (x ) around x, where f (x) is differentiable. Using equation 4.7 leads to

< f (x) > = Ω f (x) + f (x)(x -x) + r(x -x) 2 W (x -x , h) dx . (4.8)
RHS integral term in last equation is then split in three integral terms,

< f (x) > = f (x) Ω [W (x -x , h)] dx = 1 +f (x) Ω [(x -x)W (x -x , h)] dx = 0 +r(h 2 ) . (4.9)
Since kernel W is an even function meaning that

W (x -x , h) = W (x -x, h) , (4.10)
the following term (xx)W (xx , h) in RHS of equation 4.9 is an odd function. Thus, integrating this last term on a spherical domain gives zero:

Ω (x -x)W (x -x , h) dx = 0 . (4.11)
First RHS term in equation 4.9 should be equal to one, since it is derived from equation 4.6. This is called normalization condition:

Ω [W (x -x , h)] dx = 1 . (4.12)
Applying normalization condition (Eq. 4.12) and previous relation (Eq. 4.11), equation 4.9 becomes

< f (x) >= f (x) + r(h 2 ) . (4.13)
The second order accuracy of the kernel approximation hence depends on two conditions:

• The smoothing function must be an even function. Otherwise, equation 4.11 is not valid.

• The normalization condition (Eq. 4.12).

Smoothed

Integral representation of the derivative of a function

The approximation of the spatial derivative ∇f (x) is obtained simply by substituting f (x) with ∇f (x) in equation 4.7. This gives,

< ∇f (x) >= Ω [∇f (x )] W (x -x , h) dx , (4.14)
where the gradient is operated with respect to the primed coordinate x.

The term inside RHS integral,

[∇f (x )] W (x -x , h) , (4.15)
can be rewritten as follows,

∇ [f (x )W (x -x , h)] -f (x )∇W (x -x , h) . (4.16)
Inserting it in equation 4.14, one obtains,

< ∇f (x) >= Ω ∇ • [f (x )W (x -x , h)] dx - Ω f (x )∇W (x -x , h) dx . (4.17)
By applying Gauss' gradient theorem (Eq. 2.4) on the first RHS integral in equation 4.17, this term is rewritten into an integral over the surface dS which delimits the integration domain Ω,

< ∇f (x) >= S f (x )W (x -x , h) dS - Ω f (x )∇W (x -x , h) dx . (4.18)
Since the smoothing function W is defined to have compact support, when the support domain is located within the computational domain, i.e. not truncated, the surface integral on the right hand side of equation 4.18 becomes zero. Therefore, equation 4.18 is simplified as follows,

< ∇f (x) >= - Ω f (x )∇W (x -x , h) dx . (4.19)
For points whose support domain is crossing the boundaries of the domain, the surface integral term cannot be neglected in equation 4.18. Under such circumstances, modifications should be made to remedy the boundary effects if the surface integration is treated as zero in equation 4. [START_REF] Douglas | Comments on modeling interfacial flows with volume-of-fluid methods[END_REF]. The renormalizing technique is one possible remedy (see section 4.2.4.8 ).

Note that the Kernel gradient ∇W (xx , h) is an odd function, i.e.

∇W (xx , h) = -∇W (xx, h) . (4.20)

Therefore, its integration over the compact support gives,

Ω ∇W (x -x , h) dx = 0 . (4.21)
Similarly to the integral representation of a function, the integral representation of the derivative of a function is second order accurate [START_REF] Oger | Aspects théoriques de la méthode SPH et applications à l'hydrodynamique à surface libre[END_REF].

CHAPTER 4. COUPLING SPH WITH FINITE VOLUME

Particle approximation of a function and its derivatives

Infinitesimal volume dx at location of the particle j is now approached by its finite volume V j . It is related to its mass m j and volumetric mass ρ j with following simple relation:

m j = V j ρ j . (4.22)
Thus, starting from equation 4.7, the discrete expression of a function at location of the particle i is,

< f (x i ) >= N j=1 m j ρ j f (x j )W (x i -x j , h) , (4.23)
or with shorthand notation

W ij = W (x i -x j , h), < f (x i ) >= N j=1 m j ρ j f (x j )W ij . (4.24)
The same approximation may be applied on the spatial derivative of a function (Eq. 4.19):

< ∇f (x i ) >= - N j=1 m j ρ j f (x j )∇ i W ij . (4.25)
For approaching a second spatial derivative < ∇•∇f (x i ) >, different forms exist in the context of SPH. Three of them are given below. Demonstrations can be found in [START_REF] Fatehi | Error estimation in smoothed particle hydrodynamics and a new scheme for second derivatives[END_REF][START_REF] Brookshaw | A method of calculating radiative heat diffusion in particle simulations[END_REF].

• The first and natural choice consists to use two times an approximation of a first derivative. This form is named as double summation form. It is expressed as follows:

< ∇ • ∇f (x i ) >= - N j=1 m j ρ j (< ∇f (x i ) > •∇ i W ij ) . (4.26)
• The second form consists to use the second derivative of the kernel function:

< ∇ • ∇f (x i ) >= - N j=1 m j ρ j f (x j )∇ • ∇ i W ij . (4.27)
• The third and last form [START_REF] Brookshaw | A method of calculating radiative heat diffusion in particle simulations[END_REF] consists of a finite-difference-like form for the first derivation and a SPH summation for the second derivative:

< ∇ • ∇f (x i ) >= 2 N j=1 m j ρ j f (x i ) -f (x j ) x 2 ij (x ij • ∇ i W ij ) . (4.28)

Kernel functions

Properties of the Kernel functions

The smoothing or kernel function W should satisfy seven conditions [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF]:

lim h→0 W (x -x , h) = δ(x -x ) . (4.30) (iii) Compact condition: W (x -x , h) = 0 when |x -x | > κh , (4.31)
where κ is a constant related to the smoothing function which defines its effective (nonzero) area [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF].

(iv) Decay condition: The smoothing function value should be monotonically decreasing with the rise of the distance away from the particle.

(v) Positivity condition: The kernel function value should be positive within the support domain of the considered particle.

(vi) Symmetric property: W (xx , h) must be an even function so that the following symmetric property is respected,

W (x -x , h) = W (x -x, h) . ( 4.32)
(vii) Smoothness condition: The smoothing function should be sufficiently smooth.

Kernel functions families

Different smoothing functions have been proposed and tested in literature [START_REF] Jj Monaghan | Artificial viscosity for particle methods[END_REF][START_REF] Wendland | Piecewise polynomial, positive definite and compactly supported radial functions of minimal degree[END_REF][START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF][START_REF] Violeau | Fluid Mechanics and the SPH method: theory and applications[END_REF][START_REF] Yang | SPH simulation of fluid-structure interaction problems with application to hovercraft[END_REF].

• First family is Gaussian kernel family [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF][START_REF] Violeau | Fluid Mechanics and the SPH method: theory and applications[END_REF]. The simplest expression is:

W (x ij , h) = α d h d e -( x ij h ) , (4.33)
with d the number of dimensions of the system, x ij the absolute distance between the two points i and j, and α d a constant defined in such a way that the kernel function respects the normalization condition (Eq. 4.29). Values of α d for the simple Gaussian function are

α d = 1 π for d = 2 (two dimensions) , 1 π 3/2
for d = 3 (three dimensions) .

(4.34)

The Gaussian kernel is considered sufficiently smooth even for high orders of derivatives. It is very stable and accurate especially for disordered particles. It shows however a higher cost to compute than Wendland kernel functions, detailed later, for instance.

• Another popular family is B-splines functions group. These functions are written as,

W (x ij , h) = α d h d f x ij h . (4.35)
The third order B-Spline has been defined by Monaghan and Lattanzio [START_REF] Jj Monaghan | Artificial viscosity for particle methods[END_REF] as,

f (q) =      1 -3 2 q 2 + 3 4 q 3 if 0 ≤ q ≤ 1 , 1 4 (2 -q) 2 if 1 ≤ q ≤ 2 , 0
elsewhere, (4.36) where q = x ij h is the normalized distance between particles i and j, and α d is equal to 10 7π and 1 π in two and three dimensions, respectively. • Another family is the Wendland kernel function [START_REF] Wendland | Piecewise polynomial, positive definite and compactly supported radial functions of minimal degree[END_REF] defined as,

W (x ij , h) = α d h d f x ij 2h . (4.37)
Below, second and fourth order Wendland kernel functions are shown:

-Quadratic Wendland kernel function:

f (q) = (1 -q) 4 (4q + 1) , 0 if q > 2 . ( 4
f (q) = (1 -q) 6 (35q 2 + 18q + 3), 0 if q > 2. (4.39)
α d is equal to 3 4π and 165 256π respectively in 2D and 3D.

For the two previous functions, the normalized distance q is here equal to x ij 2h .

The Wendland kernel functions have the ability to avoid the tensile instability that may arise when a derivative approaches zero as two particles come near each other [START_REF] Yang | SPH simulation of fluid-structure interaction problems with application to hovercraft[END_REF].

Weakly Compressible SPH formalism

The most popular SPH method in fluid dynamics for incompressible flow is the so-called Weakly-Compressible Smoothed Particle Hydrodynamics (WCSPH) approach. This approach is based on the assumption that, for low Mach number configurations (M ≤ 0.1), the fluid is weakly-compressible, i.e. the density does not vary more than 1%, and barotropic, i.e. density is a function of pressure only. Thus, without considering the energy equation which does not play any role in an adiabatic flow, the equation system is composed of 5 equations (in 2D) or 6 equations (in 3D):

• 1 equation for density (from mass conservation) (section 4.2.4.1),

• 2 or 3 equations for velocity components (from momentum conservation) (section 4.2.4.2),

• 1 equation for pressure (state equation according to density) (section 4.2.4.4),

• 1 equation for position (from equation of motion) (section 4.2.4.3).

The advantages of this method are as follow: easy programming since the pressure is directly derived from the density through an algebraic thermodynamic equation (see section 4.2.4.4); explicit treatment of diffusion terms (see section 4.2.4.2). The drawbacks are the very small time step associated with a numerical speed of sound which is at least 10 times higher than the maximum of velocity and the artificial pressure fluctuations which can yield numerical instability [START_REF] Lee | Comparisons of weakly compressible and truly incompressible algorithms for the sph mesh free particle method[END_REF].

Particle approximation of density

A first and simple approach is the summation density, which is directly the particle approximation of the density. Replacing LHS function in equation 4.24 by density, the following equation is obtained [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF]:

ρ i = N j=1 m j W ij . (4.40)
Another approach consists to discretize the continuity equation. Starting from the continuity equation in Lagrangian form (Eq. 4.3), the particle approximation is applied on the RHS term [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF],

Dρ i Dt = -ρ i N j=1 m j ρ j U j • ∇ i W ij . (4.41)
Another form accounts for the relative velocities of particles pairs and serves to reduce errors arising from the particle inconsistency problem [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF]. This formulation is expressed as:

Dρ i Dt = ρ i N j=1 m j ρ j U ij • ∇ i W ij , ( 4.42)
with U ij = U i -U j the relative velocities.

Particle approximation of momentum

The derivation of SPH formulations for particle approximation of momentum conservation is somewhat similar to the continuity density approach. The starting point is the Lagrangian form of the momentum equation:

DU Dt = 1 ρ ∇ • σ , (4.43)
with σ the total stress tensor, expressed as,

σ = -pI + τ . (4.44)
The viscous stress tensor τ is expressed as,

τ = µ ∇U + ∇U T - 2 3 (∇ • U ) I , ( 4.45)
with I the unit vector. It is common in WCSPH method to neglect compressibility of the flow in the discretization of the equation. In that way, the divergent of the viscous stress tensor is written as,

∇ • τ = µ∆U . (4.46)
Morris et al. proposed a mix of finite-difference-like form (Eq. 4.28) and SPH summation (Eq. 4.25), that has been used later in the thesis of Cherfils [START_REF] Cherfils | Développements et applications de la méthode SPH aux écoulements visqueux à surface libre[END_REF] in hydrodynamic configurations:

DU i Dt = - N j=1 m j P i + P j ρ i ρ j ∇ i W ij - N j=1 m j 2µ ρ i ρ j x ij • ∇ i W ij x 2 ij U ij , ( 4.47)
where x ij = x i -x j is the distance between particles i and j.

Equation of motion

The simplest approach for an equation of motion, without using particle approximation, is simply the derivative of the particle position:

Dx i Dt = U i . (4.48)
Equation of motion 4.48 can also be written in XSPH formalism (see section 4.2.4.7) by adding an artificial smoothing term.

Equation of state for pressure

Since WCSPH method is considered compressible, pressure is derived from density and other constants. Following Monaghan et al. [START_REF] Joe | Simulating free surface flows with sph[END_REF], the Tait equation proposed by Batchelor [START_REF] Keith | An introduction to fluid dynamics[END_REF] to describe the change of pressure with change of density in a liquid is used as equation of state [START_REF] Vorobyev | A Smoothed Particle Hydrodynamics Method for the Simulation of Centralized Sloshing Experiments[END_REF]:

P rel = P abs -P 0 = B ρ ρ 0 γ -1 . (4.49)

Smoothed Particle Hydrodynamics 147

When considering the liquid as water, the specific heat ratio γ = 7 and the reference density ρ 0 = 1000 kg/m 3 . Usually, the reference pressure P 0 = 0 so that the relative pressure is equal to the absolute pressure. It allows to greatly simplify the treatment of free surfaces with the WCSPH method.

The constant B defines how large the change in pressure is in relative to density variation. This constant is defined as,

B = ρ 0 c 2 0 γ , (4.50)
where c 0 is the reference sound velocity. Sound velocity in water is equal to 1480 m/s. This value is very high and would involve a very small time-step during simulation because of the CFL (Courant-Friedrich-Levy) condition. Hence, an artificial sound velocity is chosen based on following relation [START_REF] Yang | SPH simulation of fluid-structure interaction problems with application to hovercraft[END_REF]:

c 2 0 = U 2 max δρ ρ = U 2 max M 2 , (4.51)
with M the Mach number and U max the bulk velocity of the fluid. A typical value for sound velocity would be 10 times the bulk velocity so that the density variation does not exceed more than 1%. WCSPH method is a pseudo-compressible method for that reason.

On the other hand, the stability of the simulation directly depends on the value of the artificial sound velocity.

Temporal discretization

Time-stepping requires the definition of the time integration discretization scheme adopted to update particle positions. Previous particle approximation equations reduces the original continuum PDEs to sets of ODEs. Then, any stable explicit time-stepping algorithm for ODEs can be used. A classical explicit or forward Euler scheme (Eq. 2.41), applied to density and momentum equations, gives:

           U n+1 i = U n i + ∆t DU Dt n i , ρ n+1 i = ρ n i + ∆t Dρ Dt n i . (4.52)
Then, using velocity values at new instant, discretized motion equation follows:

x n+1 i = x n i + ∆tU n+1 i . (4.53)
This temporal discretization scheme is simple to implement but may show a low time-step value because of the CFL constraint. Therefore, we present below two explicit Predictor-Correct time-stepping schemes, one from Liu et al. [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF] and a modified Verlet from Monaghan [START_REF] Joe | Smoothed particle hydrodynamics[END_REF].

• This predictor-corrector scheme [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF] has the advantage of easy implementing. At the first (predictor) step, velocity and density are evaluated as follows:

           U n+1/2 i = U n i + 0.5∆t DU Dt n i , ρ n+1/2 i = ρ n i + 0.5∆t Dρ Dt n i . (4.54)
Afterwards, time derivative of density is calculated, pressure is updated based on chosen equation of state and time derivative of velocity is calculated.

Corrector step consists in correcting all evolution variables (velocity, position and density) as follows:

                   U n+1 i = U n i + ∆t DU Dt n+1/2 i , x n+1 i = x n i + ∆tU n+1 i , ρ n+1 i = ρ n i + ∆t Dρ Dt n+1/2 i , (4.55)
where n,n + 1/2,n + 1 denote the values at the start, halfway and at the end of a time step, respectively.

• Modified Verlet time-stepping scheme conserves linear and angular momentum exactly [START_REF] Joe | Smoothed particle hydrodynamics[END_REF]. At the first (predictor) step, all the evolution variables are evaluated as follows:

                 U n+1/2 i = U n i + 0.5∆t DU Dt n i , x n+1/2 i = x n i + 0.5∆tU n i , ρ n+1/2 i = ρ n i + 0.5∆t Dρ Dt n i . ( 4.56)
Afterwards, pressure is updated based on chosen equation of state and time derivative of velocity is calculated.

Corrector step consists in correcting velocity and position, then in calculating density time derivative based on new values of velocity and position. Finally, density is corrected:

                   U n+1 i = U n i + ∆t DU Dt n+1/2 i , x n+1 i = x n+1/2 i + 0.5∆tU n+1 i , ρ n+1 i = ρ n+1/2 i + 0.5∆t Dρ Dt n+1 i . ( 4.57)

Treatment of boundary conditions

In/out-flow boundaries SPH has been successful in modeling unbounded (e.g. astrophysical) processes and wall-bounded unsteady flows (e.g. dam break and wavemaker flows) but it has not been widely used for problems with inflow and outflow [START_REF] Lastiwka | Permeable and non-reflecting boundary conditions in sph[END_REF]. Two types of boundaries exist in literature: periodic boundaries [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF] and buffer zone boundaries [START_REF] Federico | Simulating 2d openchannel flows through an sph model[END_REF].

Periodic boundaries

For simulating flows with imposed external forces such as a pressure gradient in the direction of the flow (Poiseuille flow or Couette flow), the most simple way to set up the inlet and outlet boundary conditions consists to apply periodic boundaries in the flow direction [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF]. This periodic condition applies both on motion and interaction of particles. Concerning particle motion, a particle that leaves the specified region through a particular boundary face immediately re-enters the region through the opposite face. Concerning particle interaction, a particle located within the dimension of the support domain from a boundary interacts with particles in an adjacent copy of the system, or equivalently with particles near the opposite boundary.

In other words, this wraparound effect of the periodic boundary condition is taken into consideration in both the integration of the equations of motion and the interaction computations between neighboring particles.

Buffer zone boundaries

Without a periodic configuration, it is necessary to define buffer zone boundaries in order to impose uniform upstream and downstream flow conditions. In the work of Federico et al. [START_REF] Federico | Simulating 2d openchannel flows through an sph model[END_REF], buffer zones with inflow and outflow particles are defined. Each particle is assigned to a set of particle:

• Fluid when it is inside fluid domain. Navier-Stokes equations govern the motion of these particles.

• Inflow when it is inside inflow buffer zone. Particles are advected with prescribed quantities.

• Outflow when it is inside outflow buffer zone. Particles are advected with previous quantities they have got before entering the buffer zone.

Between the fluid domain and buffer zones, thresholds are defined: if a particle crosses these thresholds, it changes the set the particle belongs to. For instance, an inflow particle that crosses the limit with fluid domain becomes a fluid particle and evolves in accordance with the WCSPH equations.

At the inflow, the desired velocity and pressure conditions are assigned to the inflow particles.

Their are distributed on a regular grid and move according to their velocity. At the outflow, an open-boundary condition is prescribed: the fluid particles that cross the outflow threshold become outflow particles. Their physical variables do not evolve in time any more with the exception of their positions that evolve according to the particle velocities. They are frozen particles [START_REF] Federico | Simulating 2d openchannel flows through an sph model[END_REF].

For both buffer zones, creation and deletion of particles is performed at the end of each time step. Their thickness must be as wide as the kernel radius to avoid truncation of the fluid particles kernel.

Solid wall modeling

Two approaches for modeling walls with SPH can be found in literature:

(i) Dummy particles [START_REF] Violeau | Fluid Mechanics and the SPH method: theory and applications[END_REF] or fixed ghost particles, (ii) Mirror [START_REF] Violeau | Fluid Mechanics and the SPH method: theory and applications[END_REF] or Virtual [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF] particles.

(i) The dummy particles are established as a network of evenly spaced stationary particles, arranged in several layers beyond the edge particles. The number of layers should be sufficient so that the kernel support of a particle close to the wall is not truncated. This particles are considered as "dead" since their related quantities are constant over time. They affect the density of the fluid particles lying near the wall.

In [START_REF] Cherfils | Développements et applications de la méthode SPH aux écoulements visqueux à surface libre[END_REF], Cherfils updates the pressure and density properties of the particles in the first layer of the wall in accordance with the SPH continuity equation and the state equation. The pressure and density properties in other layers are copied from this first layer.

(ii) The mirror particles are a variant of the previous dummy particles. The difference lies in the fact they are reconstructed upon each time iteration. The procedure consists in adding -to each fluid particle c close enough to the wall-a mirror particle m provided with parameters which are symmetric to those of c. They have same pressure and density but different velocity. Velocity is opposite in normal direction for a wall slip condition:

U m • t = U c • t , U m • n = -U c • n , ( 4.58)
with t and n the tangential and normal unit vectors to the wall respectively. Velocity is opposite in both normal and tangential directions for a no slip condition:

U m • t = -U c • t , U m • n = -U c • n , (4.59)
An illustration of these mirror particles is shown in figure 4.2. One of the advantages in this procedure is that a no-slip condition can more easily and accurately be achieved with mirror particles than dummy particles. This method is favorably simple but at the cost of extra computational time and additional memory space [START_REF] Violeau | Fluid Mechanics and the SPH method: theory and applications[END_REF]. Ghost particles (red) are mirrored from the fluid particles (blue) to enforce: on the left a no-slip boundary condition and on the right a free slip boundary condition.

U m U c U m U c

Stabilizing techniques

WCSPH formalism uses centered operators in an explicitly solved system and consequently such a formalism is unconditionally unstable [START_REF] Afonso | Improvement of the precision and the efficiency of the SPH method: theoretical and numerical study[END_REF]. One common numerical phenomenon in

Smoothed Particle Hydrodynamics

151

SPH is the so-called "tensile instability" [START_REF] Cherfils | Développements et applications de la méthode SPH aux écoulements visqueux à surface libre[END_REF]: particles group together by small packages in zones of the flow where they are compressed by the pressure. In order to restore stability, it is necessary to add some numerical diffusion. In the literature, such a technique is often referred as up-winding. Each up-winding scheme originates a different WCSPH variant. Different variants are briefly described in the following sub-parts.

Artificial viscosity

As in other numerical methods, an artificial viscosity can be added to a viscousness model, in order to improve numerical stability. Momentum equation is then modified, by the adding of a term Π ij that is homogeneous to a pressure term. This artificial term was developed by Monaghan et al. [START_REF] Joe | Simulating free surface flows with sph[END_REF] to allow shocks to be simulated with WCSPH.

Diffusive terms in the continuity equations

Diffusive term methods help eliminating a large part of the numerical noise affecting the evaluation of ρ and, consequently of p [START_REF] Antuono | Free-surface flows solved by means of sph schemes with numerical diffusive terms[END_REF]. Therefore, it helps to get rid of the non-physical pressure oscillations and to get a smooth pressure distribution. Here, two variants of the diffusive term D i to be added into the continuity equation 4.42 are proposed. SPH-approached continuity equation 4.42 with introduction of this term is expressed as follows,

Dρ i Dt = ρ i N j=1 m j ρ j U ij • ∇ i W ij + D i . ( 4.60)
The definition of diffusive term D i is given by

D i = N j=1 ψ ij x ij |x ij | • ∇ i W ij m j ρ j . ( 4.61)
The term ψ ij is defined differently, depending on the considered SPH-variant, i.e. δ-SPH or Rusanov-flux:

• The Rusanov flux has been developed by Ferrari et al. [START_REF] Ferrari | A new 3d parallel sph scheme for free surface flows[END_REF] in 2009. In this method, ψ ij is defined as,

ψ ij = c ij (ρ j -ρ i ) , (4.62)
with c ij = max(c i , c j ) the sound celerity, that can be calculated with the following equation of state [START_REF] Cherfils | Développements et applications de la méthode SPH aux écoulements visqueux à surface libre[END_REF]:

c i = c 0 ρ i ρ 0 3 . ( 4.63)
• The δ-SPH has been proposed by Antuono et al. [START_REF] Antuono | Free-surface flows solved by means of sph schemes with numerical diffusive terms[END_REF]. The term ψ ij is expressed here with an intensity coefficient ξ whose value is customizable:

ψ ij = ξc 0 h 2(ρ j -ρ i ) |x ij | . ( 4.64)
Additionally, standard δ-SPH also combines an artificial viscosity term added in the momentum equation.

On one hand, with the Rusanov flux approach, it is not necessary to setup an intensity coefficient for the diffusive term and it does not introduce additional diffusion. On the other hand, δ-SPH includes an additional viscosity term in the momentum equation which has the advantage to improve further the pressure distribution but has the drawback to not conserve energy [START_REF] Lu | Sph numerical computations of wave impact onto a vertical wall[END_REF].

Extended SPH (XSPH)

The XSPH technique was introduced by Monaghan [START_REF] Joe | Simulating free surface flows with sph[END_REF] and consists to add an average velocity term, either in the equation of motion 4.65, either directly to the velocity [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF]. In both ways, the particle arrangement becomes more ordered and prevent the unphysical penetration of particles through each other. Adding the XSPH term directly to velocity has the advantages to smooth the velocity profiles and to avoid non-physical velocity oscillation in the flow [START_REF] Cherfils | Développements et applications de la méthode SPH aux écoulements visqueux à surface libre[END_REF]. An equation of motion 4.2.4.3 with XSPH formalism is expressed as [START_REF] Vorobyev | A Smoothed Particle Hydrodynamics Method for the Simulation of Centralized Sloshing Experiments[END_REF],

Dx i Dt = U i + N j=1 m j ρ ij U ji W ij , (4.65)
where U ji = U j -U i , ρ ij the average density of the interacting pair of particles (i -j) and a tune parameter between 0 and 1. The smallest value of , ensuring stability of the numerical solution without adding too much artificial diffusion, should be chosen [START_REF] Vorobyev | A Smoothed Particle Hydrodynamics Method for the Simulation of Centralized Sloshing Experiments[END_REF].

Density smoothing by Mean Least Square (MLS)

In the SPH method, each particle has a fixed mass m j .Thus, as long as the number of particles is constant, mass conservation is intrinsically satisfied. However, by using the evolution equation 4.42 for the density, consistency between mass, density and occupied area cannot be enforced as it would be possible by using summation density [START_REF] Colagrossi | Numerical simulation of interfacial flows by smoothed particle hydrodynamics[END_REF]:

ρ i = N j=1 m j W ij . ( 4.66)
Thus to alleviate this problem, the density field is periodically re-initialized by applying the previous equation. However, when the normalization condition (Eq. 4.29) is not respected along interfaces, free surfaces or boundaries, the use of equation 4.66 would introduce additional errors.

Hence, Belytschko [START_REF] Belytschko | On the completeness of meshfree particle methods[END_REF] proposed a density smoothing approach with corrected Kernel values, ensuring the normalization condition.

A correct frequency for re-initialization may be every 20 time-steps.

Renormalization of the kernel

The kernel function (Eq. 4.7) can furnish inaccurate results if the normalization condition 4.29 is not respected, for instance when the kernel support is truncated by a boundary condition or when particle repartition is inhomogeneous. Using a normalized core can restore that condition [START_REF] Bonet | Variational and momentum preservation aspects of smooth particle hydrodynamic formulations[END_REF][START_REF] Pw Randles | Smoothed particle hydrodynamics: some recent improvements and applications[END_REF]. It consists in defining a new kernel function Wij as,

Wij = ω i W ij = W ij N j=1 m j ρ j W ij . ( 4.67)
With this method, the theoretical second order accuracy of the kernel function is not reached but a first order accuracy is respected whatever the particle arrangement. This correction requires an additional loop over the particles for computing the weight coefficient ω i .

Renormalization of gradients

As for the kernel approximation of a function, the kernel approximation of a gradient can lose accuracy once the particle arrangement inside the kernel support is not homogeneous. One re-normalization technique has been introduced by Vila in 1996 [START_REF] Vila | Méthodes particulaires régularisées. développements récents et nouvelles applications[END_REF] then Lanson and Vila [START_REF] Lanson | Meshless methods for conservation laws[END_REF] and will be presented here [START_REF] Cherfils | Développements et applications de la méthode SPH aux écoulements visqueux à surface libre[END_REF].

The goal is, as for core correction, to restore values of the first order discrete moments of the core gradient, in order to the improve the interpolations accuracy. These moments are written, for a particle i, in the discrete form, as,

N j=1 m j ρ j x ji ⊗ ∇W ij . ( 4.68)
Following the methodology of Eldredge et al [START_REF] Jeff D Eldredge | A general deterministic treatment of derivatives in particle methods[END_REF], these moments should theoretically take as value an identity matrix I of size 2 × 2 and 3 × 3 in two and three dimensions respectively. This condition is not always fulfilled, close to truncated boundaries or in homogeneous zones. Therefore, a way to restore these values is to use a renormalized matrix L i in order to obtain:

N j=1 m j ρ j x ji ⊗ (L i ∇W ij ) = I . ( 4.69)
This matrix takes the following form in two dimensions:

L i =   N j=1 m j ρ j (x j -x i )∇ x W ij N j=1 m j ρ j (x j -x i )∇ y W ij N j=1 m j ρ j (y j -y i )∇ x W ij N j=1 m j ρ j (y j -y i )∇ y W ij   -1 . ( 4.70)
This correction should be applied in SPH conservation equations in which the kernel gradient is used.

Variable smoothing length

The smoothing length h is very important in the SPH method. It has a direct influence on the efficiency of the computation and the accuracy of the solution [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF]. Considering a scaling factor κ = 2 (κh being the kernel support radius) and a smoothing length of 1.2 times the particle spacing, the number of neighboring particles, excluding the considered one, should be 4, 20 and 56 in one, two and three dimensions respectively. In inhomogeneous zones, this number may not be reached. A way to keep it relatively constant is to use a variable smoothing length h i that varies according to local conditions. Several expressions of h i can be found in [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF]. However, with such method, additional terms which account for the variability of the smoothing lengths should be included in the SPH equations in order to satisfy conservation requirements. It is also more complex to setup a linked-list algorithm in neighboring particles search algorithm.

Neighboring Particles search algorithm

The Nearest Neighboring Particles Searching (NNPS) consists to list the particles j inside the Kernel support of a given particle i, for the whole set of particles. Two different ways of searching are briefly described below [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF]:

• The most simplest way, so-called All-pair search algorithm consists, for a given particle i, to calculate the distance x ij from i to each and every particle j inside the whole domain.

When this distance falls below the kernel support κh, particle j is added as a neighbor. The computational cost of this method is proportional to N 2 , N being the total number of particles in the domain. This method is simple but obviously expensive. The second method highly reduces this computational effort.

• Considering a constant smoothing length, the most cheapest way is the so-called Linkedlist algorithm [START_REF] Vorobyev | A Smoothed Particle Hydrodynamics Method for the Simulation of Centralized Sloshing Experiments[END_REF]; the cost of order of this method is proportional to N . As the influence of neighbors stops outside the kernel support, a Cartesian grid is set up whose cells size is linked to the smoothing length, i.e. 2h. Each particle receives the cell index in which it lies. In this way, the nearest particles can be known by considering only the direct neighboring cells.

Validations

Preliminary investigations of the potential of the Weakly Compressible SPH (WCSPH) method have been performed with a in-house code. These investigations serve as a basis before implementation of WCSPH in OpenFOAM R library and the later coupling with finite volume method. This in-house code has been developed in C++, based on the Fortran algorithm detailed in the book of Liu et al. [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF].

In this section, we show validation of the In-House WCSPH solver over two simple test cases. First, a Poiseuille flow configuration, in which an analytical solution is known, allowing to validate the SPH model, more particularly the treatment of the viscous term. Second, a laminar jet in a coflow, based on work of Aristodemo et al. , that allows to validate the buffer zone open boundary conditions that are inlet and outlet.

Poiseuille flow

Test case details

Poiseuille flow is a simple configuration that is well adapted to validate modeling of the viscous effects with the SPH solver. It consists in a laminar flow between two fixed plates situated above and below flow domain. The initially steady fluid is driven by a body force F , gradually accelerates between the two plates and finally arrives at a steady state.

The Poiseuille flow is defined with the following characteristics:

• Geometric characteristics:

Channel length: L = 5 × 10 -4 m.

Channel high: l = 1 × 10 -3 m.

• Flow characteristics:

Kinetic viscosity: water viscosity, ν = 10 -6 m 2 /s.

Density: water density, ρ = 10 3 kg/m 3 .

Driven body force, equivalent to a pressure gradient divided by density:

F = 1 ρ ∂P ∂x = 2 × 10 -4 m/s 2 . ( 4.71)
Analytical solution for a steady state Poiseuille flow is:

U x (z) = F 2ν z(z -l) . ( 4.72)
The peak fluid velocity or bulk velocity is obtained for z = l 2 . With the given kinetic viscosity and driven body force, it gives U max = 2.5×10 -5 m/s. The corresponding low Reynolds number is Re = 2.5 × 10 -2 according to its definition:

Re = U max × l ν . ( 4.73)

Computational conditions

We chose here to impose the body force as an external force, included as an acceleration source term in the velocity equation. Therefore, periodic conditions are imposed in the streamwise direction.

The simulation is built with the following SPH characteristics and parameters:

• Equation system:

Mass conservation: equation 4.42.

Momentum conservation: equation 4.47.

Equation of motion: equation 4.48.

State's equation for pressure: equation 4.49.

• Boundary conditions:

Inlet and outlet: Periodic conditions (see section 4.2.4.6).

Walls: Ghost Particles (applying no-slip conditions) (see section 4.2.4.6).

• Kernel's function: A simple Gaussian kernel is chosen for its accuracy (Eq. 4.33).

• Stabilizing technique: None. The validation case is a Low Reynolds number case. Thus, it is not necessary to add some artificial diffusions or any stabilizing techniques since the flow is stable.

• Temporal discretization: Predictor-corrector (equations 4.54 and 4.55).

800 particles are used (20 in x-streamwise-direction times 40 in y-spanwise-direction). The initial conditions are null velocity and null pressure in the whole computational domain. The time-step is defined with the following relation, considering CFL conditions both for convection [START_REF] Violeau | Fluid Mechanics and the SPH method: theory and applications[END_REF] and viscous diffusion [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF]:

∆t = min 2.33 h c 0 , 0.125 h 2 ν , ( 4.74)
with c 0 the initial speed velocity, calculated with the relation 4.51,

c 2 0 = U 2 max δρ ρ , ( 4.75)
where density variation δρ ρ is set to 1%. In the current viscous configuration, the time step value is equal to 1.4 × 10 -4 s, which is imposed by the viscous term in equation 4.74. The simulation reaches a steady state at t = 0.6 s. The smoothing length used is set as 1.33 times the initial particle spacing [START_REF] Cherfils | Développements et applications de la méthode SPH aux écoulements visqueux à surface libre[END_REF] in order to obtain the required number of 20 neighboring particles. Velocity is nondimensionalized by the bulk velocity located at the center on the duct.

Results

Velocity field is shown in figure 4.4. It shows an homogeneous repartition of the particles as well as an homogeneous velocity field, that is not impacted by the periodic boundary conditions. As shown in the axial velocity profiles of SPH and analytical solutions in figure 4.3, SPH results are in very good agreement with the analytical solution, since the relative error is less than 0.32%.

Laminar jet in a coflow

This test case deals with a 2D horizontal jet injected in a coflowing environment. It has been used by Aristodemo et al. [START_REF] Aristodemo | Sph modeling of plane jets into water bodies through an inflow/outflow algorithm[END_REF] for applying a SPH inflow/outflow algorithm. We chose to reproduce this numerical simulation with our SPH solver for the same reason, i.e. apply inflow/outflow buffer zones (see section 4.2.4.6). Furthermore, it is a simple configuration with injection of one phase into another which can be exploited later for an hybrid SPH/Finite Volume coupled solver (see section 4.6).

Test case details

D B L U 1 U 0 jet centerline

Computational conditions

The simulation is built with the following SPH characteristics and parameters:

•

• Boundary conditions:

Inlet and outlet: Inlet/Outlet boundary conditions [START_REF] Federico | Simulating 2d openchannel flows through an sph model[END_REF] (see section 4.2.4.6).

Walls: Ghost Particles (applying slip conditions) (see section 4.2.4.6).

• Kernel's function: Gaussian function (Eq. 4.33).

• Stabilizing technique: A diffusive term is added into the continuity equation with flux

Rusanov variant [START_REF] Ferrari | A new 3d parallel sph scheme for free surface flows[END_REF], in order to smooth the pressure field.

• Temporal discretization: Predictor-corrector (equations 4.54 and 4.55).

• Neighboring particle search: Linked-list algorithm (part 4.2.4.9).

Final system of PDEs is as follows:

                                   Dρ i Dt = ρ i N j=1 m j ρ j U ij • ∇ i W ij + D i , DU i Dt = - N j=1 m j P i + P j ρ i ρ j ∇ i W ij - N j=1 m j 2µ ρ i ρ j x ij • ∇ i W ij x 2 ij U ij , P i = P 0 + B ρ i ρ 0 γ -1 , Dx i Dt = U i , (4.76)
with diffusive term D i expressed as,

D i = N j=1 ψ ij n ij • ∇ i W ij m j ρ j , (4.77)
where

n ij = x ij x ij , ( 4.78)
and,

ψ ij = c ij (ρ j -ρ i ) , (4.79)
with c ij = max(c i , c j ) the sound celerity. It is calculated with the following equation of state [START_REF] Cherfils | Développements et applications de la méthode SPH aux écoulements visqueux à surface libre[END_REF]:

c i = c 0 ρ i ρ 0 3 . (4.80)
20000 fluid particles are used (200 in x-streamwise-direction times 100 in y-spanwise-direction), i.e. a resolution of 25 particles for one diameter, plus ghost particles for modeling walls (2 layers on each walls, 808 particles average), plus inflow particles and outflow particles (2 times 400 particles). The initial conditions are U (t = 0, x) = U 0 and P (t = 0, x) = 0. The time-step is defined with the following relation, considering CFL conditions both for convection [START_REF] Cherfils | Développements et applications de la méthode SPH aux écoulements visqueux à surface libre[END_REF] and viscous diffusion [START_REF] Liu | Smoothed particle hydrodynamics: a meshfree particle method[END_REF]:

∆t = min β h c 0 , 0.125 h 2 ν , ( 4.81)
with chosen CFL condition β = 0.3 and c 0 the initial speed velocity, calculated with the relation 4.51,

c 2 0 = U 2 1 δρ ρ , ( 4.82)
where density variation δρ ρ is set to 1%. The smoothing length used is set as 1.33 times the initial particle spacing [START_REF] Cherfils | Développements et applications de la méthode SPH aux écoulements visqueux à surface libre[END_REF] in order to obtain the required 20 neighboring particles. Therefore, the time step, constrained by CFL condition for convection, is equal to 1.33 × 10 -3 s. The simulation reaches a steady state after 22 s.

Zero velocity and pressure gradients are enforced to avoid the generation of flow perturbations at the outlet. Null pressure is assigned at the inlet.

Results

Qualitative results

Evolution of phase going out from inlet is shown in figure 4.6. For t (U 1 /D) = 3, the jet tip is subjected to an initial shape deformation due to a relevant velocity gradient induced by the excess velocity between jet and current. In the successive transitory instants (t (U 1 /D) = [8, 10.5]), the jet shows a larger deformation of its initial part, showing a growth of a not well developed vortex pair [START_REF] Aristodemo | Sph modeling of plane jets into water bodies through an inflow/outflow algorithm[END_REF].

Comparison with finite volume

Weakly Compressible SPH Results are compared with those of a finite volume single-phase incompressible solver: icoFoam solver from OpenFOAM R library. A Cartesian mesh with a similar resolution (200×100 cells) is chosen for the domain discretization. Boundary conditions are similar, i.e. Dirichlet conditions for pressure and velocity at inlet. Pressure is also imposed along the walls in this incompressible formalism.

Inherent asset of Lagrangian methods for tracking interface is here shown by comparing SPH and FV fields respectively in figures 4.6 and 4.7. The Lagrangian method shows a sharp interface between the inlet and coflow phases (respectively black and grey particles) while the Eulerian method shows some diffusion of the jet tip during the whole transient state, from t (U 1 /D) = 3 to t (U 1 /D) = 10.5. The diffused zone thickness increases along with the development of the jet tip. This is due to the Eulerian treatment of the convection term, see equation 4.89 for instance. More details about the transport of a passive scalar will be given in next part 4.6 about coupling SPH and FV methods.

Evolutions of axial and transverse velocity profiles are shown respectively in figures 4.8 and 4.9.

During transient state at instant t (U 1 /D) = 10.5, SPH profile values are similar to those of FV profile, without being equal, due to the weakly compressible formalism of SPH. Jet tip penetrations (peak value) are identical. To improve the correspondence between SPH and FV results, a density-based weakly compressible FV solver should be run instead of an incompressible solver.

Nevertheless, both simulations reach closely the same steady state profile as shown in figures 4.8-(b) and 4.9-(b).

Regarding computational cost, SPH simulation requires 29 times more CPU effort than FV simulation, for the same CFL constraint (0.3) and domain discretization resolution. This important ratio is mainly due to the explicit and compressible formalisms of the SPH model, increasing the CFL constraint. This cost can be lowered by reconsidering the frequency of call of the NNPS algorithm, the kernel function (a Wendland function could be cheaper than a Gaussian function) and the memory storage of particle tributes [START_REF] Braun | Hpc predictions of primary atomization with sph: Challenges and lessons learned[END_REF].

Increase of velocity ratio.

Previous configuration is a reproduction of Aristodemo et al. work [START_REF] Aristodemo | Sph modeling of plane jets into water bodies through an inflow/outflow algorithm[END_REF] using different SPH equations. It has shown a good agreement between SPH results and incompressible finite volume results with a slower convergence rate to steady state though. We have tried then to change the conditions of this test case towards a higher velocity gradient between inlet and coflow streams. Current velocity ratio is U 1 /U 0 = 1.5. For a velocity ratio U 1 /U 0 = 5, U 1 = 0.05 m/s, CFL condition β = 0.3 and ∆t = 4 × 10 -4 s, results are negative. Simulation diverges after t (U 1 /D) = 0.45 due to instabilities. Despite reduction of the time step, instability problems remain. One also observes particles deficiency inside the vortexes enclosing the jet tip. To remedy to these issue, an investigation of different SPH equations and stabilizing techniques should be performed as well as an increase of the particle resolution. However, because of the computational cost of SPH, we did not pursue our efforts. Instead, we focused on developing finite volumes coupling. Black and grey particles stand respectively for inlet and coflow particles. Diffusion induced by the numerical method is shown in blue and brown.

Coupling of SPH with FV methods: Literature review

In the following section, a short review of the existing works about coupling SPH with FV methods are presented. Each work is organized by the type of Domain Decomposition Method (DDM) that is used, i.e. either grid patching, overlapping grids or grid superposition (see part 3.2.2 for more details about DDM). A chronology of these works is shown in figure 4.10.

Coupling through grid patching:

• In the thesis of Barcorolo [START_REF] Afonso | Improvement of the precision and the efficiency of the SPH method: theoretical and numerical study[END_REF], coupling algorithm between a SPH-ALE scheme and a Voronoi-FV scheme using an auxiliary mesh for the SPH domain, is presented. The goal of the coupling is to treat free surfaces with SPH while the more precise FV scheme is used for the large fluid domain. The Voronoi-FV is a Arbitrary Lagrange Euler (ALE) method, based on Voronoi meshes [START_REF] Aurenhammer | Voronoi diagrams-a survey of a fundamental geometric data structure[END_REF], where nodal location (free to move at each time step) serves as generator point for a Voronoi region and results in a Control Volume (generated at each time step). Weakly-compressible Navier-Stokes equations are solved in both domains. The interaction between the two distinct numerical domains is made through a neat interface, hence a grid patching-type DDM. Two methods for treating fluxes at the interface are proposed:

-Conservative approach: It consists to compute fluxes for every face of the SPH-FV interface. Then, these fluxes are adapted with the normal flux method [START_REF] De Leffe | Normal flux method at the boundary for sph[END_REF][START_REF] De | Modelisation d'ecoulements visqueux par methode sph en vue d'application {à} l'hydrodynamique navale[END_REF].

Fluxes have to be added in correct quantities so that instabilities are not generated in the SPH domain.

-Simplest but non-conservative approach: SPH particles are treated as Voronoi Finite Volumes neighbors and Voronoi volume centroids as SPH particles neighbors. In other words, no special treatment is done for computing fluxes at the interface. This method is thus non-conservative due to the different level of accuracy of the SPH and FV operators.

In order to separate the fluid domain into the SPH and FV sub-domains, it is necessary to perform a free-surface detection. This is done by applying the method proposed by Marrone et al. [START_REF] Marrone | Fast freesurface detection and level-set function definition in sph solvers[END_REF] for the semi-implicit ISPH algorithm used in [START_REF] Afonso | Improvement of the precision and the efficiency of the SPH method: theoretical and numerical study[END_REF]. The drawback of this coupling approach is that it requires computation of an auxiliary mesh: a Voronoi tessellation is constructed on the whole fluid domain at each time step.

Coupling through grid overlapping:

• The thesis of Mancip in 2001 [START_REF] Mancip | Couplage de méthodes numériques pour les lois de conservation[END_REF] is the first work in our knowledge about SPH-FV coupling. Its work is applied on an injection problem, where the cold chamber in upstream is modeled using FV while the next chamber including the jet is modeled using SPH. • In the work of Bouscasse et al. [START_REF] Bouscasse | Multi-purpose interfaces for coupling sph with other solvers[END_REF], SPH is coupled with a FV solver and this procedure is validated on a standing wave test case. The finite volume solver relies on an incompressible implicit scheme while the SPH solver is in Weakly-Compressible form and explicit in time. The SPH field boundary conditions are imposed through a "ghost fluid region" composed by fully Lagrangian particles. They cover the whole interface region and evolve according to the field given by the external solution (the FV solver). The physical quantities necessary in the SPH integration scheme are obtained through a Mean Least Square (MLS) interpolation of the FV field.

• The work of Marrone et al. [START_REF] Marrone | Coupling of smoothed particle hydrodynamics with finite volume method for free-surface flows[END_REF] is in the continuity of the previous work of Bouscasse et al. . A SPH/FV coupling scheme is employed here for modeling a breaking wave. SPH method is chosen close to the free surface in order to capture pressure peaks thanks to the weakly compressible model, whereas a FV method is dedicated to the main body of the flow field where compressibility plays a minor role. Both mathematical models are weakly compressible Navier-Stokes equations. However, because the FV time step is much larger than what is required to capture compressibility effects, the FV solver tends to an incompressible solver [START_REF] Marrone | Coupling of smoothed particle hydrodynamics with finite volume method for free-surface flows[END_REF]. SPH time integration is explicit with a time step smaller than the FV time step, while FV time integration is implicit. Thus, SPH domain is subcycled in time compared to Finite Volume domain. In terms of computational costs, the coupled solution was at least ten times faster than the solutions obtainable by the two separate approaches.

• The most recent work which has been founded dedicated to SPH/FV coupling for treating free surfaces is the one from Gianguzzi [START_REF] Gianguzzi | An hybrid finite volumesph method for incompressible flows[END_REF]. Applied on standing and propagating wave problems, the coupling scheme guarantees a smooth transition between the solutions in the FV and SPH domains by the introduction of a layer of grid cells in the SPH domain and a band of virtual particles in the FV one (both neighbouring the interface). Solution is obtained through suitable interpolation procedures from the local solutions.

• In 2014, Neuhauser [START_REF] Neuhauser | Development of a coupled SPH-ALE/Finite Volume method for the simulation of transient flows in hydraulic machines[END_REF] publishes a thesis about SPH-FV coupling in order to simulate transient flows in hydraulic machines. Both FV and SPH solvers are weakly compressible and explicit in time. The transfer of information from SPH particles to FV boundary Cells is performed with a Shepard interpolation [START_REF] Shepard | A two-dimensional interpolation function for irregularly-spaced data[END_REF] scheme. The scalar φ c located at a cell center is interpolated from quantities φ j of the neighbouring SPH particles j inside the kernel support of the FV cell:

φ c = j φ j m j ρ j W cj k m k ρ k W ck . ( 4.83)
This interpolation on cell values is not mass conservative, meaning that mass is lost or gain in the process. Mass unbalance needs to be evaluated so it can be recovered.

Coupling by grids superposition:

• The work of McCue-Weil et al. , published in 2012 [START_REF] Kumar | Coupled SPH-FVM Simulation within the OpenFOAM Framework[END_REF], deals also with free surfaces problems. On one hand, it aims to exploit the strength of SPH to manage free surfaces, deformable boundaries, moving interfaces or large deformations. On the other hand, it aims to avoid its drawback to deal with boundary conditions and its heavy computational cost. Therefore, SPH is used only near free surfaces (see figure 4.11) whereas the gridbased FV method is used in the rest of the domain.

The FV method is a two-phase VOF method, that is interFoam solver of the OpenFOAM R framework. The nature of the VOF method means that an interface between the species is not explicitly computed, but rather emerges as a property of the phase fraction field. Since the phase fraction can have any value between 0 and 1, the interface is never sharply defined, but occupies a volume around the region where a sharp interface should exist.

In short, McCue-Weil et al. [START_REF] Kumar | Coupled SPH-FVM Simulation within the OpenFOAM Framework[END_REF] aim to capture liquid-gas interface with SPH and to correct its position and curvature in the VOF field.

Solutions of each solver are merged such as the SPH solution replaces the FV results at the interface. Using a dedicated algorithm, the SPH domain is constructed on interfacial regions defined by cells with phrase fraction 0 < α < 1 or cells with strong gradients of α. At each time step, the algorithm principle is as follow:

1 Whole FV domain solution is advanced for one time-step using single grid interFoam solver. 4 Velocity values in interfacial FV cells are replaced by interfacial SPH particle values using integral interpolation smoothed via kernel function.

Their validation is based on a two phase dam-break case. The results are mitigated: the numerical results show poor agreement with the experimental data due to the 3D nature of the dam break that is not taken in account in their simulation, and the computational cost is impacted by the use of the SPH method.

Numerical scheme of the coupling

The coupling strategy between SPH and FV methods proposedin this thesis is based on the previous zonal method (see section 3.4), on ghost particles boundary type and existing meshless interpolation schemes. For the sake of simplicity in this first attempt of SPH/FV coupling, zonal and global domains will be run with same time-step. In other words, subcycling in time is not considered.

The considered coupling algorithm for a single phase laminar flow, with transport of a passive scalar γ, illustrated in figure 4.12, is as follow:

(1) Solve entirely GD, for one global ∆t time step, using FV single grid solver algorithm.

(2) Prolongation step: Velocity of ghost particles in coupled boundary conditions of ZD is updated based on interpolation in space of GD solution.

(3) Solve entirely ZD, for one zonal ∆t time step, using single grid solver algorithm.

(4) Restriction step: ZD velocity and passive scalar fields are transferred to GD through Shepard interpolation.

Face flux restriction is not performed since, (i) the SPH velocity field is not divergence free due to the weakly compressible formalism, and (ii) as shown in the work of Neuhauser [START_REF] Neuhauser | Development of a coupled SPH-ALE/Finite Volume method for the simulation of transient flows in hydraulic machines[END_REF], meshless interpolations are not mass conservative.

Furthermore, it can be noticed that this coupling is passive: no correction step is performed after restriction step. Finite Volume scheme is incompressible, with a segregated approach for the resolution of the pressure-velocity coupling. Therefore, after the restriction step of velocity from ZD to GD, a correction step should be performed to update pressure and face fluxes based on this new velocity values.

Thus, there is room to improve this coupling scheme. The purpose of this first numerical scheme is to test and show the potential of coupling a fully Lagrangian solver with an Eulerian one.

Prolongation step

Coupled boundary conditions for velocity in zonal domain are Dirichlet. It is based on ghost particles whose positions and properties are determined from internal fluid particles: the procedure consists in adding to each fluid particle close enough to the wall a mirror particle which is the symmetric relative to the boundary face (see figure 4.2 for illustration). Pressure, density and passive scalar of both particles are identical. Here, at the difference of a classical wall boundary condition, ghost particle velocity is interpolated from underlying cell values. Interpolation is performed in one step, at the contrary of the FV-FV coupling where interpolation is decomposed in normal and tangential interpolation. We chose to employed an Inverse Distance Weighting (IDW) interpolation, because this scheme is part of the available OpenFOAM R library interpolations. Velocity of ghost particle g is expressed as, where superscript N stands for number of closest points in FV mesh to the particle position, here four, and subscript k stands for one of the four points. A point is either a cell vertex, i.e. a corner, either a face center, either a cell centroid. The interpolation weight ω k is defined as,

U g = N k ω k U k N k ω k , ( 4
ω k = 1 |d k,g | , ( 4.85)
where |d k,g | is the distance between the particle g and the point k.

Restriction step

Correction of FV velocity and passive scalar fields are performed in the restriction step. The values that are corrected are inside cells overlaid by the SPH zonal domain. Concerning the interpolation, scattered data approximation techniques are well adapted since SPH particles are an unstructured cloud of points. Moving least square (MLS) approximation of any order can be chosen. In our configuration, a Shepard interpolation is employed [START_REF] Shepard | A two-dimensional interpolation function for irregularly-spaced data[END_REF]. Corrected value of arbitrary field φ in a covered cell P is expressed as follows,

φ P = N j ω j φ j j k ω j , ( 4.86)
where subscript j stands for a neighbor SPH particle and superscript N is the number of particles inside the kernel of cell centroid P . The interpolation weight ω j is defined as,

ω j = m j ρ j W P,j , (4.87)
where W P,j is the kernel value based on the distance between the centroid P and the particle j position.

In order to know which particles are inside the P cell kernel and obtain them from the SPH cloud, the linked-list grid is used. The linked list grid is part of the neighboring particles search algorithm. For a given particle, the nearest particles can be known by considering only the direct neighboring cells. In our coupling, the connectivity between the GD and ZD cells is established prior to simulation. Therefore, in the restriction step, for each covered cell in GD, one gets its neighbor particles by considering the cloud occupancy inside each neighbor ZD cells.

To avoid numerical instabilities caused by the ghost particles at the Neumann condition outlet boundary in SPH zone, the neighboring ZD cells along this boundary are not considered in the restriction process.

Zonal domain inflow and outflow

The coupled boundary conditions allow to manage outflow: when a fluid particle crosses the delimitation between SPH fluid domain and the buffer zone, it is automatically deleted. However, it does not allows to manage inflow: if the flux is going inside the zonal domain, we do not consider in the current coupling scheme the generation of particles. This comes from the acknowledged difficulty of the SPH method to handle the mass inflows. Indeed, for a uniform velocity profile, as the inlet physical boundary condition, it is straightforward to insert particles with a prescribed velocity. In literature, inlet boundary condition consists to create ghost particles upstream from inlet patch and to let advecting them into fluid domain. Mass inflow is respected. On the other hand, for non-uniform and time varying velocity profile, it is more complex to handle. Nevertheless, this issue has been investigated in literature and possible solutions exist. In the work of Kassiotis [START_REF] Kassiotis | Semi-analytical conditions for open boundaries in smoothed particle hydrodynamics[END_REF] et al. , particles are generated based on a mass flux computed at the wall. It consists to create a particle when accumulated mass on a face becomes greater than a threshold value. Accumulated mass flux is then reseted by subtracting the new particle mass from accumulated mass value. This method has been then improved by Chiron [START_REF] Chiron | Couplage et améliorations de la méthode SPH pour traiter des écoulements à multi-échelles temporelles et spatiales[END_REF] in his thesis: particle generation is placed at the middle of coupled patch faces instead of patch vertexes.

Application on plane jet in a coflow with transport of a passive scalar

∂γ ∂t + 1 V f (γ f F ) = 0 . ( 4.90)
It thus involves face interpolation and consequently numerical diffusion. Objective of such coupling is thus to correct γ field in the FV domain with a zonal SPH domain phase field.

To setup the numerical methods coupling, a Weakly Compressible SPH (WCSPH) solver has been implemented in the OpenFOAM R library. As a reminder, OpenFOAM R is a C++ toolbox for the development of customized numerical solvers for the solution of continuum mechanics problems, including computational fluid dynamics (CFD). The code is released as free and open source software. It offers a wide range of finite volume solvers, from single to two-phase and from laminar to turbulent flows. However, it does not include any SPH method, hence the necessary developments have been performed by Nicolas Hecht at the laboratory "Laboratoire Ondes et Milieux Complexes" in Le Havre, France.

Computational conditions

Rectangular channel flow with length L = 10D and height B = 5D is the overall domain in which finite volume method will be used. Sub-domain in which SPH method will be utilized is sized to l = 5D and b = 3D and placed close to injector inlet (see figure 4.13) whose diameter D = 0.01 m. Liquid is injected inside the domain through injector with a time-constant horizontal velocity U 1 = 1.5U 0 . Velocity U 0 refers to the velocity of the steady current above and below injector, whose value is U 0 = 0.01 m/s. The flow is laminar since Reynolds number is Re = 500.

The keakly compressible SPH solver, discretization schemes and kernel employed in this configuration are the same than in the previous single SPH simulation shown in part 4.3.2.

Zonal Domain

Global Domain Concerning discretization of the divergence term in equation (4.90) with the FV solver, a Gauss linear scheme is chosen for its second order accuracy. The boundary conditions are identical to those employed in part 4.3.2, i.e. null pressure and velocities are imposed at the inlet.

D B = 5D L = 10D U 1 U 0 l = 5D b = 3D

Transport of a scalar in finite volume

Prior to the SPH-FV coupling, three different mesh refinements are tested in Finite Volume, without coupling, as shown in It can be observed that head of the jet is diffused (brown color) even with the finer mesh.

Only fine mesh field shows a distinctive jet head, with a "mushroom-head" shape. To reduce the diffusion of γ, it is therefore necessary either to refine again the mesh, thus increasing the computational cost, either to correct the field with a Lagrangian formalism, hence the SPH-FV coupling.

The next SPH-FV simulation will be performed using the fine refinement in FV mesh.

SPH-FV coupling results

Refinement between FV mesh and SPH particles is set to r x = 2.5: 2.5 times more particles are present in the zonal region than in the finite volume cells. It leads to a total number of SPH fluid particles in the zonal domain of 24k. Convective CFL condition is set to 0.3 in SPH domain. With relation (4.81), it leads to a constant time-step ∆t SP H = 0.64 ms. In FV domain, with a convective CFL condition set to 0.5, it leads to a constant time-step ∆t F V = 21 ms. Thus, if time sub-cycling was applied, the time-step ratio between these two time-steps should be r t = 32. In this configuration, time sub-cycling is not applied. Therefore, FV time-step is enforced to SPH time-step value.

Computational cost of the FV resolution is anyway far lower than the SPH cost.

The simulation is run until tU/D = 15. In the lower part of figures (2), the corrected FV field shows a lower diffusion from tU/D = 2 to tU/D = 6. The head jet shape is in close accordance with the SPH shape and the thickness of the diffusion part, i.e. γ ∈ [0, 0.5] (brown color in figure 4. [START_REF] Paul | The computer simulation of dispersed two-phase flow[END_REF], is reduced in comparison with the FV field with no correction. The remaining diffusion is due to the Shepard interpolation process and, in a lesser measure, the visualization interpolation.

After tU/D = 6, the zonal domain has not anymore influence on the head of the jet (figures (2.d) and (2.e)). The head jet conserves a more compact aspect with a thiner diffusion zone in comparison with the uncorrected FV fields ((1.d) and (1.e)).

Computational costs

Computational cost of a SPH and FV simulations alone has been addressed in previous part 4.3.2.3. SPH simulation requires 29 times more effort than a single FV run for the same CFL constraint and same domain discretization resolution.

In this part dealing with a SPH/FV coupling, the CPU effort with the zonal SPH correction is increased by a factor of 10 in comparison with a single FV run with same CFL constraint and same domain discretization resolution, i.e. counting 2.5 2 times more cells. It is thus currently not worth regarding the computational cost to use a SPH zonal correction. However, the purpose of this study was to show the feasibility of such a coupling, and the interest regarding the transport of a scalar. Several options can be considered to reduce SPH single grid solver CPU cost: an incompressible SPH method will allow to reduce the time-step ; the neighboring particle search algorithm can be optimized by reducing the call frequency, let's say every 20 time-steps ; smaller smoothing lengths; relaxed CFL conditions; optimizing the memory allocation of particle lists; a Wendland kernel function could be cheaper than a Gauss function.

Summary and discussion

This chapter presented an adaptation of the zonal methodology described in Chapter 3 to couple a zonal Smoothed Particle Hydrodynamics (SPH) domain with a global finite volume domain.

This method has been applied on a laminar single phase two dimensional test case, in which a jet transporting a passive scalar is injected into a steady current.

The SPH method is able to describe the interface between the jet tip and the steady current very accurately without diffusion of the transported scalar, thanks to its Lagrangian nature.

The coupling process is able to transfer this description from the SPH domain to the finite volume domain, hence reducing the diffusion of the interface in the latter domain. Thus, this method shows a great potential for two phase flows, in which an accurate description of the interface is primordial.

The velocity coupling needs however further investigations in order to accommodate the difference between the two numerical methods, as the boundary conditions and the incompressiblecompressible formalisms. Furthermore, to extend this coupled approach to more complex and two-phase flow configurations, three major challenges have to be addressed:

• First and most important challenge concerns the computational cost. SPH method is known to be costly, due to its compressible and explicit formulations. In this thesis, a new SPH solver has been implemented inside OpenFOAM R library. For this reason, the solver is at a early stage and can be optimized in the future regarding computational cost.

In the literature, Braun et al. [START_REF] Braun | Hpc predictions of primary atomization with sph: Challenges and lessons learned[END_REF] have shown that the performance of the method can be highly improved, with gains up to the order of 5, by using less expensive kernel functions, smaller smoothing lengths, relaxed CFL conditions and by optimizing the memory allocation of particle lists.

• Second challenge concerns the stability of the method. It has been shown in the preliminary validation part, that instabilities and particle deficiencies, due to high velocity gradients, may lead to the divergence of the simulation. This problem is highlighted in [START_REF] Safdari | Improved multiphase smoothed particle hydrodynamics[END_REF]. However, in these series of work [START_REF] Braun | Modeling fuel injection in gas turbines using the meshless smoothed particle hydrodynamics method[END_REF][START_REF] Braun | Hpc predictions of primary atomization with sph: Challenges and lessons learned[END_REF][START_REF] Koch | Prediction of primary atomization using smoothed particle hydrodynamics[END_REF], the authors show that the SPH method, despite its premature stage, is able to simulate complex two-phase flow configurations and a primary atomization process.

• Third and last challenge concerns boundary conditions. In this work, inflow and outflow boundary conditions have been used based on the work of [START_REF] Federico | Simulating 2d openchannel flows through an sph model[END_REF][START_REF] Aristodemo | Sph modeling of plane jets into water bodies through an inflow/outflow algorithm[END_REF]. These buffer zones allow to remedy the limitation of SPH by the lack of suitable open boundary conditions [START_REF] Braun | Modeling fuel injection in gas turbines using the meshless smoothed particle hydrodynamics method[END_REF]. It is however not sufficient for dealing with mixed inflow-outflow boundaries, in which the fluid goes in and out at different locations. This type of boundary is essential for coupling a zonal domain with a global one. In the work of Kassiotis et al. [START_REF] Kassiotis | Semi-analytical conditions for open boundaries in smoothed particle hydrodynamics[END_REF], a technique, in which particles are generated based on a mass flux computed at the boundary, has been proposed and may represent a solution to this issue.

Chapter 5

Application to numerical simulation of primary atomization

Introduction

As a reminder, the main goal of this thesis is to address multiscale and multiphysic issues of the atomization process by developing an hybrid method that divides the flowfield into two zones: a inner zone dedicated to solve the primary atomization region and a outer zone for the rest of the field including the dispersed spray region.

In previous chapters, this zonal methodology was developed, based on existing Adaptive Mesh Refinements (AMR) and Domain Decomposition Methods (DDM), validated on simple two dimensional test cases, and at last parallelized.

In this chapter, we apply this flow solver to predict the primary breakup of a single cylindrical liquid jet in an airblast atomizer configuration. Numerical results will be compared with experimental results from [START_REF] Stepowski | Measurement of the liquid volume fraction and its statistical distribution in the near development field of a spray[END_REF]. This test case has been chosen for three reasons: (i) Experimental data are available about the mean volume fraction in the primary atomization region; (ii) liquid and gas Reynolds numbers are relatively low in comparison with pressure atomizer configurations, limiting the computational cost; (iii) it seems pertinent to use two different two phase flow models in this configuration. In the near nozzle field, a VOF method (RI model) will effectively capture the interface instabilities and liquid structures detachments. A fine resolution will thus be necessary. In the far field, a Eulerian/Lagrangian Spray Atomization (ELSA) method (TDF model) will be able to treat low volume fractions of the liquid that has been atomized and dispersed. The configuration being turbulent, a Large Eddy Simulation (LES) turbulent model will be employed to model the smallest eddies of the flow.

With this application, we wish to measure the performance gain between this zonal approach and a "standard" simulation. Parallel performance of the zonal solver will be also investigated. Furthermore, it is important that the zonal methodology does not degrade the accuracy of one of the two phase flow models. Numerical results, of both zonal and standard simulations, will be compared to experimental results. Finally, mass conservation of the zonal solver will be checked and discussed. PRIMARY ATOMIZATION

In the following, a simulation using the zonal grid approach is referred to as a zonal simulation and a simulation using a single mesh and a single two phase solver is referred to as a standard simulation.

Application case details

The considered configuration, issued from Stepowski et al. [START_REF] Stepowski | Measurement of the liquid volume fraction and its statistical distribution in the near development field of a spray[END_REF], consists of injecting a low-speed liquid through a circular pipe and a high-speed gas through an annular pipe into a steady atmosphere. The liquid used is pure water, and ambient gas is dry air, leading to a density ratio of approximately 1000. The sketch of the injector is presented in figure 5.1. The 2 kg/m 3 , U l = 1.3 m/s, ρ l = 1000 kg/m 3 . To obtain the near field of liquid volume fraction, α, the fluorescence emission of an additional specie incorporated into the water induced by a pulsed laser sheet has been used [START_REF] Stepowski | Measurement of the liquid volume fraction and its statistical distribution in the near development field of a spray[END_REF]. Surface tension coefficient σ is derived from aerodynamic Weber number, defined as,

D l D g ∆ Liquid : U l , ρ l Gas : U g , ρ g
W e g = ρ g (U g -U l ) 2 D l σ .
(5.1)

Gas and liquid Reynolds numbers, respectively expressed as,

Re g = ρ g U g (D g -D l -2∆) µ g , ( 5.2)
and

Re l = ρ l U l D l µ l , ( 5.3)
are high enough so that turbulent flows may be expected. Momentum flux ratio J, expressed as,

J = ρ g U 2 g ρ l U 2 l , ( 5

Computational conditions

Turbulence model

LES (Large Eddy Simulation) [START_REF] Stephen B Pope | Turbulent flows[END_REF] is based on the idea of computing the large, energy-containing eddy structures which are resolved on the computational grid, whereas the smaller, more isotropic, sub-grid structures (SGS) are modeled. Large structures are isolated by a filter operation. The filter width is taken as the cube root of the local grid cell volume. The effect of the small scales is obtained through the sub-grid scale stress term that must be modeled.

The WALE (Wall-Adapting Local Eddy-viscosity) model [START_REF] Nicoud | Subgrid-scale stress modelling based on the square of the velocity gradient tensor[END_REF] is used in this paper. This LES model recovers the proper near-wall scaling for the eddy viscosity without requiring dynamic procedure. Moreover, the WALE model is invariant to any coordinate translation or rotation and no test-filtering operation is needed. It is therefore well adapted for this injector case, where walls enclose both gas and liquid inlets. As a last benefit, this model does not need to solve an additional scalar transport equation. Hence, no additional variable coupling is necessary between global and zonal domains.

Computation domain and mesh

The global computational domain is defined as a cylindrical mesh with a height of 16D l and a diameter of 8D l , as shown in figure 5.2. Small inner portion of the pipe is modeled, whose length is equal to 0.1D l , and allows to account grossly for wall boundary layer, especially with liquid inlet where laminar conditions are specified.

An expanding mesh is used to focus refinement efforts in a region of size

[-0.1D l , 3D l ] × [-1.1D l , 1.1D l ] × [-1.1D l , 1.
1D l ] that cover primary and secondary atomization areas. Three different mesh refinements will be used in the simulations. One coarse refinement to reduce computational cost. One medium refinement to obtain correct predictive results regarding the mean liquid volume fraction in the primary atomization region, with a reasonable computational cost. Finally, one fine refinement to get accurate predictive results. These three mesh refinements are shown in figure 5.3 with a front view of the discretized liquid inlet. The number of cells at liquid nozzle exit and the cell size both at liquid and gas nozzles are shown in table 5.2.

Without considering the liquid atomization but only the turbulent flow leaving gas pipe, the medium mesh refinement is sufficiently fine to capture vortexes with LES. Indeed, the following PRIMARY ATOMIZATION estimation for the minimal LES mesh resolution ∆ x is recommended by Addad et al. [START_REF] Addad | Optimal unstructured meshing for large eddy simulations[END_REF]: ∆ x = max (λ g , l/10) , (5.5) where λ g and l are respectively Taylor micro-scale and turbulent length scale at gas nozzle exit. These two characteristic lengths can be estimated respectively with following relations [START_REF] Stephen B Pope | Turbulent flows[END_REF][START_REF] Henk | An introduction to computational fluid dynamics: the finite volume method[END_REF]:

D l 8D l 16D l 4D l
λ g = √ 10Re -1/2 l l , ( 5.6
)

l = 0.07D h , ( 5.7)
with D h = D g -(D l + 2∆) the hydraulic diameter and Re l the turbulence Reynolds number specific to the turbulent length scale:

Re l = k 1/2 l ν , ( 5.8)
where k is the turbulent kinetic energy. Further from the nozzle, the turbulent length scale and the Reynolds number are estimated based on a posteriori known spray cone diameter and mean velocity magnitude. 5.2: Mesh refinement at the gas and liquid nozzle exits, along with the number of cells in radial direction at liquid nozzle exit.

but it is downstream at 3D l with a minimum cell size ∆ x | 3D l = 169µm. Thus, it justifies the use of a coarse mesh to reduce computational in zonal simulations as detailed later. Now, regarding the liquid atomization, it will be shown later that medium and fine refinements respectively procure correct and accurate estimations of the mean liquid penetration, with an ICM model.

When using coarse mesh refinement, the cell-to-cell expansion ratio, after the refined region previously mentioned, is about 1.05 in axial direction and 1.1 in radial direction, which is an acceptable limit regarding mesh quality.

Velocity is imposed with Dirichlet boundary conditions at gas and liquid inlets. It is set to zero value along the walls and an inlet-outlet boundary condition, which is a mixed Dirichlet-Neumann type, is applied on the atmospheric boundary condition. Total pressure is specified on atmospheric boundary condition with a reference value of 0. Other boundary conditions are Neumann conditions with zero gradient specified. Volume fraction value is fixed to 1 in liquid inlet and to 0 in gas inlet. Zero gradient is applied along the wall and a inlet-outlet boundary condition is applied on the atmospheric boundary condition. Finally, eddy viscosity ν t which is a calculated value in the internal field, does not need to be specified or corrected on wall boundaries. Zero gradient conditions are applied all along the boundaries.

Initial conditions are at rest for the whole domain with null velocity and atmospheric pressure. Liquid pipe is filled with water. An adaptive time step is used, constraint by a maximum CFL condition equal to 0.5. Subcycling on volume fraction advection resolution is also performed, with a time ratio of 2.

Gas inlet

Gas Reynolds number Re g = 8000 shows the turbulent character of the flow. It is shown in the work of Xiao et al. [START_REF] Xiao | Les of turbulent liquid jet primary breakup in turbulent coaxial air flow[END_REF] in which LES of similar atomization configurations are performed, that the initial interface perturbations caused by liquid and gas eddies plays an important role in the resulting surface instability development and primary breakup process. When turbulent inflows were specified, they predict correctly experimental core breakup lengths. Their flow conditions show momentum flux ratio J varying between 0.17 and 2 . In the present paper, simulated configuration shows a momentum flux ratio with a value of 10. One can thus assume that gas eddies will have a great impact on the interface disturbance and that gas unsteady turbulent inlet velocity conditions should be specified.

To do so, the decaying turbulence inflow generator developed by Kornev et al. [START_REF] Kornev | Synthesis of artificial turbulent fields with prescribed second-order statistics using the random-spot method[END_REF][START_REF] Kornev | Synthesis of homogeneous anisotropic turbulent fields with prescribed second-order statistics by the random spots method[END_REF] is PRIMARY ATOMIZATION used. The velocity field is represented as the sum of velocities induced by a set of randomly distributed spots. Velocity distribution inside of each spot is found in such a way that the fluctuations possess prescribed statistical properties. These statistical properties are mean gas velocity U g , turbulent length scale l and the six components of the symmetric Reynolds-stress tensor, expressed for a round jet as [START_REF] Stephen B Pope | Turbulent flows[END_REF],

   u 2 uv 0 uv v 2 0 0 0 w 2    .
(5.9)

Due to the anisotropic but predictable turbulent character of a round jet flow, the four unknown components u 2 , v 2 , w 2 and uv , are linked together with the following relation [START_REF] Stephen B Pope | Turbulent flows[END_REF]:

u 2 = 2 v 2 = 2 w 2 = 4 uv .
(5.10)

First Reynold stress term u 2 is derived from the turbulent kinetic energy k:

u 2 = 2 3 k . (5.11)
Rough approximation for the inlet distribution of k is obtained from the turbulent intensity T i and the inflow velocity [START_REF] Henk | An introduction to computational fluid dynamics: the finite volume method[END_REF]:

k = 2 3 (U g T i ) 2 .
(5.12)

Scaling expression for the turbulence intensity as a function of the Reynolds number in a smooth pipe is used [START_REF] Russo | Scaling of turbulence intensity for low-speed flow in smooth pipes[END_REF]: T i = 0.14 × Re -0.079 g .

(5.13)

Finally, the last statistical property to prescribe is the turbulent length scale l. A commonly used relation for flow in smooth pipes is [START_REF] Henk | An introduction to computational fluid dynamics: the finite volume method[END_REF]:

l = 0.07D h . (5.14)
Despite a high mesh refinement regarding Taylor length scale based estimation, as previously mentioned, it is commonly admitted that the biggest eddies should be modeled with at least 5 cells, to avoid numerical decay of turbulent structures. Using the medium or fine mesh refinements does not allow to fulfill this prerequisite. Instead of increasing the mesh refinement, we chose to increase the turbulent length scale in order to keep turbulent structures of decaying downstream the gas inlet. The turbulent length scale l value, input data for the turbulence inflow generator, is hence set to 0.42D h and to 0.21D h for medium and fine mesh refinements respectively.

Liquid inlet

In the work of Tian et al. [START_REF] Xiu-Shan Tian | Threedimensional large eddy simulation of round liquid jet primary breakup in coaxial gas flow using the vof method[END_REF], a criterion parameter K was defined to assess the relative importance of liquid inlet velocity distributions on the liquid breakup shape of a selected atomizer:

K = δ 0 ∆ , ( 5.15)
where ∆ is the central tube thickness and δ 0 is the liquid initial vorticity thickness at the nozzle exit. For pipe flows, vorticity thickness is defined as [START_REF] Marmottant | On spray formation[END_REF],

δ 0 = cD l Re -1/2 l , ( 5.16)
where the coefficient c depend on nozzle design. Marmottant and Villermaux [START_REF] Marmottant | On spray formation[END_REF] studied the boundary layer in a axisymmetric nozzle and determined that the value of c is approximately 5.6. From the previous formulations and assumptions, a criterion value of 0.8 is found. In [START_REF] Xiu-Shan Tian | Threedimensional large eddy simulation of round liquid jet primary breakup in coaxial gas flow using the vof method[END_REF], small and large K cases are considered for criterion values of 0.3 and 2.4 respectively. It is shown that a uniform velocity distribution is suitable in the small K cases while an exponential velocity distribution is suitable in the large ones. In the current configuration, with K = 0.8, we consider being closer to a small K case than to a large one. Therefore, a uniform velocity distribution is prescribed to liquid inlet. It also allows to be strictly conservative regarding liquid mass flow rate.

Zonal simulation schemes

In the zonal schemes, primary and secondary regions are refined with a zonal domain

[-0.1D l , 3D l ]× [-2D l , 2D l ] × [-2D l , 2D l ],
as shown in yellow in figure 5.2. The length of this zonal domain, equal to 3D l , is chosen based on the experimental profile of mean liquid volume fraction along the jet center line. As shown in figure 5.12, it is approximatively equal to 0.1 at x = 3D l . This value is often considered as the transition value between separated and dispersed two phase flow zones [START_REF] Ishii | Thermo-fluid dynamics of two-phase flow[END_REF]. Therefore, it is pertinent to switch from RI to TDF model at this longitudinal location. Diameter of the zonal domain, equal to 4D l , has been chosen to avoid high gradients of velocity and liquid volume fraction along the zonal-global interface. It is thus based on preliminary observations.

Coarse mesh refinement will be used in the global domain to reduce impact of the mesh refinement in the dispersed spray zone on the computational cost. As previously mentioned, the cell size is estimated sufficiently small for LES in the uncovered part, i.e. after 3D l , based on the Taylor micro-scale equation 5.6. Zonal Domain (ZD) is refined in time and space compared to Global Domain (GD). The space PRIMARY ATOMIZATION and time ratio between GD and ZD are respectively referred to as r x and r t . In the following simulations, two space refinement will be applied: global coarse coupled with a medium zone (r x = 2) and global coarse coupled with a fine zone (r x = 4). Zonal time step ∆τ is subcycled compared to global time step ∆t by a time refinement ratio 1 ≤ r t ≤ r x that is adapted in function of CFL constraint.

Variables that are coupled in the prolongation step (from global field to zonal interface Γ) are pressure P rgh , velocity U and volume fraction α. Coupled Dirichlet boundary conditions are used for pressure along the global-zonal interface Γ, while coupled inlet-outlet conditions are used for velocity and volume fractions: when flux is going inside ZD, Dirichlet condition is applied while when flux is going out, normal gradient, that is interpolated from underlying GD face, is imposed. See part 3. RI model (VOF method), whose discretized equations are described in part 3.3, will be used in ZD. TDF model (ELSA method), whose discretized equations are described also in part 3.3, will be used in GD.

The following schemes are used for the prolongation step:

• Cell center to face center interpolation scheme for liquid volume fraction α is TDF model flux interpolation equation 3.78:

(α) f = ρF -F × ρ 2 -F ν,α × (ρ 1 -ρ 2 ) F × (ρ 1 -ρ 2 ) .
For velocity, flux corrected linear interpolation from equation 3.51 is used:

U f = Ū f + F |S| -Ū f • n f n f ,
where n f is the face normal vector and Ū f is a linear interpolation from cell centers to face centers using equation 3.57.

For pressure, a linear interpolation is performed using equation 3.57.

• Time interpolation of the three variables U , P rgh , α is a first order linear interpolation using equation :

φ(t + k∆τ ) = φ(t) + k r t (φ(t + ∆t) -φ(t)) ,
where k is the zonal subcycling iteration.

• Tangential interpolation scheme for the three variables is a first order accurate injection scheme (Eq. 3.61). With this zonal grid approach, two meshes are overlapped. The unsteady gas inflow, previously detailed, is imposed in Zonal Domain (ZD). To ensure conservation of gas inflow in both domains, inlet boundary condition in GD is mapped from ZD one. Theoretical gas mass flow rate is respected in both domains as shown in figure 5.4.

Parallel scaling tests

Before proceeding to parallel transient simulations, parallel speedup tests are performed using the Curie super-computer center [172], to run each simulation with an optimal number of processors. It also provides an estimation of the performance gains between a single mesh (standard) simulation and a coupled (zonal) simulation.

Three simulations are performed:

• One using a single mesh with medium refinement that counts 2.1M cells (referred to as medium in figure 5.5).

• A simulation using a global mesh with coarse refinement, that counts 260k cells, and a zonal mesh with medium refinement, that counts 690k cells (referred to as medium zonal in figure 5.5).

• A simulation using the same global coarse mesh than previously, and a 5.5M cells zonal mesh with fine refinement (referred to as fine zonal in figure 5.5).

In these simulations, the two phase model that is used, i.e. RI or TDF model, is not detailed in this scaling study since both have the same algorithm structure and thus quasi identical parallel performances. PRIMARY ATOMIZATION For parallelization of the CFD simulations, OpenFOAM R employs patch grids domain decomposition method. The meshes are decomposed using a simple geometric decomposition algorithm in which the domain is split into pieces by direction. The simulations are performed on the Curie super-computer [172] using Curie thin nodes. Any node is composed of two sockets containing each an 2.7 GHz Intel Sandy Bridge with 8 cores. Each core offers 64 GB of memory. The nodes are interconnected by InfiniBand QDR Network. The scaling tests are performed on a range between 1 and 96 CPU cores concerning medium effective refinement and between 1 and 240 CPU Cores concerning fine effective refinement. Each test runs from t = 0 s to t = 1.2 × 10 -6 s using adaptive time steps (CFL constraint set up to 0.5). The computational time is evaluated between starting and ending of time loop, to eliminate the influence of initialization routines and I/O during loading of the mesh from the storage device.

The results of the strong scaling tests are plotted in figure 5.5 with (a) -CPU time and (b) -efficiency. CPU Time graph (a) shows first that the medium zonal simulation is faster than medium one. For 32 processors, the gain is 63% for this short time lapse, i.e. a speed up of 2.7. In second, graph (b) shows that the efficiency of the medium zonal simulation stalls after 32 cores below 0.5. Efficiency of the medium simulation has same tendency but stalls further, after 96 cores. The next simulations with a medium effective mesh refinement will thus be proceeded using 32 cores, with parallel efficiencies respectively equal to 0.65 and 0.75. The fact that the medium zonal simulation stalls before the medium one may be due to two reasons: (i) most of the CPU effort is in the resolution of the zonal grid solver and (ii) zonal medium mesh counts less cells than the single medium mesh (692k and 2.1M respectively). Parallel efficiency decreases when mean number of cells per processor is below a certain limit. In OpenFOAM R , this limit is known to be approximatively 20k cells per processor. As a consequence, this limit is reached earlier with the smaller zonal mesh than with the large global mesh.

Performed simulations 189

Fine zonal simulation shows good scaling and a correct efficiency until 240 cores. Next zonal simulation with a fine effective mesh refinement will thus be proceeded using this amount of processors.

Performed simulations

Six different LES of the coaxial atomization configuration from Stepowski et al. [START_REF] Stepowski | Measurement of the liquid volume fraction and its statistical distribution in the near development field of a spray[END_REF] Brown, red and blue text colors respectively stand for coarse, medium and fine mesh refinements. RI and TDF models respectively stand for Resolved Interface and Turbulent Diffusive Flux models.

Four standard simulations are run using a single mesh and a single two-phase model. Coarse and medium mesh refinement as well as RI and TDF models are switched in order to highlight their influences over results. Two other simulations are performed using a global mesh and a zonal mesh, with adequate two-phase model in each mesh, i.e. RI model in zonal domain near the injector and TDF model in global domain in the dispersed spray area. The mesh refinement is increased in the zonal mesh, from medium to fine, in order to improves results quality.

Experimental data consists of volume fraction mean field, obtained with 2500 independent samples [START_REF] Stepowski | Measurement of the liquid volume fraction and its statistical distribution in the near development field of a spray[END_REF]. In our numerical simulations, mean fields are obtained by averaging at each timestep. 2). It can be observed that penetration of isocontour α = 0.5 in global domain is not much higher than in zonal domain. Indeed, it is due to (i) the physical diffusive effect of the TDF model that occurs downward ZD interface, and (ii) the numerical diffusion effect induced by the coarse mesh. It can be also seen that the interpolation process from the fine zonal mesh to the underlying coarse mesh smooths the liquid core but keep the same topology. Increasing mesh refinement in the primary atomization area leads to a more important number of smaller droplets, as shown in figure 5.8-(b.1). Pressure role is also visible.

Adequacy of the two-phase flow models

TDF model is a ELSA-based model [START_REF] Vallet | Modélisation eulerienne de l'atomisation d'un jet liquide[END_REF] that should treat as well a spherical droplet in the dispersed spray region as the distorted liquid core in the primary atomization region. It is based on the assumption that turbulence is supposed to be the mechanism leading to the detachment of liquid structure in the secondary atomization region. As a consequence, turbulence model is of primordial importance for correctly predicting the detachments of liquid structures. TDF model is shown to be unadapted for treating atomization in the primary and secondary zones, as shown mean liquid volume fraction axial profiles in figure 5.9. With coarse and medium mesh refinements, TDF model profiles are far from experimental profile. Turbulence is not enough to destabilize and provoke detachment of liquid structures. One plausible explication is that the employed LES model is a single-phase turbulent model, that is unadapted to small scales of liquid gas interface. A two-phase LES model combined with ELSA model could better predict correct liquid core length.

On the other hand, medium profile obtained with RI model that capture liquid interfaces with a VOF approach shows a correct agreement with experimental liquid penetration. Mesh refinement shows great influence over the results since coarse RI profile is as far from experimental profile than TDF profiles. Therefore, in this coaxial atomization configuration, RI model is an appropriate model for treating the primary and secondary zones.

However, it can be shown that RI model is unadapted in the further dispersed spray zone with a medium mesh refinement. In figures 5.11-(b) and 5.10-(b) are shown respectively mean and instant liquid volume fraction PRIMARY ATOMIZATION fields using RI model in the whole computational domain (medium RI configuration). We focus our following observations on the dispersed spray region, that is located grossly after 3D l , i.e. in the second half of the figures. In the instant field, it is observed that after 3D l isolated liquid droplets are not correctly captured by the method. The isocontour α = 0.5 is a relevant marker of resolved structures. This isocontour is absent due to the mesh that numerically diffuse droplets. The compressive scheme of the RI model also keep unresolved droplets to be smaller than the cell size they are advected in. In comparison, the instant medium TDF field (figure 5.10-(a)) shows a more important diffused behavior that is here not numerical but physical, induced by the model. The mesh refinement has less influence on the dispersed spray flow. Furthermore, in the mean medium RI α field (figure 5.11-(b)), lack of convergence is observed in the dispersed spray area. In comparison, for the same time period, the medium TDF field (figure 5.11-(a)) is correctly converged.

As a conclusion, the RI model is adapted in the primary and secondary atomization areas with at least a medium mesh refinement while the TDF model is adapted in the dispersed spray region. The proposed multi-approach method can combine advantages of both RI and TDF models in the dense and dispersed regions respectively. First, it can be seen, in the near nozzle region, that the medium zonal RI field is in good agreement with the medium RI field (respectively figures 5.11-(c) and 5.11-(b)). Liquid cores own very similar shape. They are also of the same length. This indicates that the coupling approach does not influence or very weakly the mean behavior of the flow in the zonal domain.

Liquid volume fraction in primary and secondary atomization regions

Second, regarding the liquid core length, at the exception of the medium TDF field (figure 5.11-(a)), the three RI fields (medium RI, medium zonal RI and fine zonal RI ) show good agreement with the experimental field (figure 5.11-(e)). However, experimental liquid core shape is here more spherical, due to repeating flapping in radial directions. This shape is not observed with numerical simulations where it tends to a conic shape with the finest mesh (figure 5.11-(d)). Insufficient convergence in time may be an explanation; one can expect to catch this shape with a longer period of simulated time. Another explanation may be the influence of the small inner walls before the nozzle exit.

Nevertheless, this flapping behavior can be observed with an instant snapshot of liquid core: A juxtaposition is made in figure 5.14 of (a) an experimental instant shot realized with fluorescence emission and (b) the isosurface of α = 0.5 obtained with the fine zonal RI configuration. The isocontour is cut at x = 3D l when zonal grid is ending. Both liquid cores show a curved surface in the lower part induced by the axial gas stream, similar to the flapping of wind-forced flags. Refining the mesh close to the nozzle gives results closer to the experimental data. With the fine zonal RI configuration, the liquid core penetration is accurately predicted in axial profile as well as liquid volume fraction peaks in radial profiles. Radial decreasing however is not catch. This tendency to decrease expresses a conic shape with fine zonal RI simulation while it expresses a spherical shape with experiment measurements, as shown above in qualitative results (figures 5.11-(d) and 5.11-(e)). As explained previously, the spherical shape is due to repeating flapping behavior, which is captured with numerical but convergence seems insufficient. RI and TDF stand for resolved interface and turbulent diffusive flux models respectively.

Zonal approach influence

It has been seen previously that, regarding the mean volume fraction values, the zonal approach provides results in good agreement with both standard simulations and experimental results.

In this section, we now discuss the influence of the zonal approach over the numerical results.

The zonal model captures liquid-gas interface using VOF approach. It is quite a meshdependent method since a sufficiently fine mesh is necessary to follow and accurately capture the smallest structures, as previously shown with the instant α field obtained with medium RI configuration (figure In TDF model, interface density Σ is followed in addition with volume fraction α. Interface density is defined as the quantity of interface area per volume control. In case of Finite Volume method, it is therefore expressed as : Σ = Interface area Cell volume .

(5.17)

This variable may treat as well a spherical droplet in the dispersed spray region as the deformed liquid core in the primary atomization region. In the TDF solver employed in this study, Σ has not any influence over the flow, it is a passive scalar transported by the flow.

Figure 5.15 shows the mean interface density field (in the global coarse mesh), obtained with the fine zonal RI simulation. Higher values are observed in the primary and secondary atomization regions, covered by the zonal domain, than in the rest of the domain. These higher values are induced artificially by the interpolation process of α from ZD to GD. Indeed, in the zonal part, interface is captured and correctly solved by RI model, i.e. α is roughly 0 or 1, without considering numerical diffusion. Volume fraction values are then interpolated to underlying coarse mesh in GD. The interpolation process diffuse the values of α and as a consequence, Σ values arise. Thus, interpolating fields from a resolved interface method fine mesh to a turbulent diffusion flux method coarse mesh has here a visible influence on one of the flow variables.

Mass conservation

It is of crucial importance to conserve liquid mass in simulations, and hence the liquid volume error in any method applied on primary atomization should be as low as possible. This particular aspect is therefore examined in the medium zonal RI simulation. Zonal domain interface Γ is shown with white lines.

When it was judged that the initial transient period is over, e.g. tU l /D l = 3.25, the following three quantities were calculated from the GD results: the liquid volume injected into the domain at inlet during a time period t V in (t), the liquid volume flowing out of the domain V out (t) and the liquid volume in the domain at time t ∆V (t) = V (t) -V (0). The first two quantities were computed from surface integrals of the liquid volume fraction on the domain boundaries and the third quantity by a volume integral within the domain.

If liquid mass is strictly conserved, the following relation should be satisfied:

V in (t) = V out (t) + ∆V (t).

(5.18)

Figure 5.16-(a) shows the evolution of these three quantities, plus the sum V out (t) + ∆V (t), for a period of 1.5tU l /D l . Since the liquid mass influx is constant, V in (t) grows linearly with time. However, the rate of liquid volume exiting the simulation varies due to turbulent fluctuations and flapping of the liquid jet. It is observed in figure 5.16-(a) that the calculated value of V out (t) + ∆V (t) matches V in (t) with an error of 0.4% after 1.5tU l /D l of simulation. It demonstrates that liquid mass is correctly conserved with our zonal approach. This value could even be lowered if a zero gradient scheme was employed as Neumann condition in the coupled inlet-outlet boundary condition of α in ZD, instead of a coupled gradient scheme. This influence was demonstrated in a parameter study of the third chapter 3.5.3.4.

In order to examine the influence of the phase volume correction step of GD cells along coarsefine interface (see section 3

Performance gains

The purpose of the two phase zonal approach is dual: switch from one two phase model to another and to gain computational time in comparison with a standard simulation. It has been shown previously in graph 5.5-(a) a good parallel scalability of the zonal method solver, similar to the one of a single grid solver in OpenFOAM R . When using 32 processors, the performance gain, between the medium zonal RI and medium RI simulations, is measured to 63% with a very short time lapse (1.2 µs), i.e. a speed up of 2.7. After simulations, the same performance gain is measured on a longer time lapse of 10 ms, as shown in table 5

Estimation of gains

The medium zonal RI and medium RI simulations have been proceeded with same environment and parameters: they are developed in the same library (OpenFOAM R ), use similar space and time discretization schemes, similar number of PISO loops, similar tolerances, etc... Hence, the only differences between these two simulations are the number of cells in each mesh, n c , and the mean time step ∆t. We propose to estimate the gain between these two simulations by using the ratio n c /∆t. The computational cost of the medium RI simulation is proportional to this ratio, while the one of the medium zonal RI simulation is proportional to the sum of the ratio of the two meshes, global and zonal.

In table 5.5-(a) is reported an estimated gain between medium zonal RI and medium RI simulations of 62%, with 1 processor. It must now be compared with the measured gain. Using 32 processors, computational gain is measured at 58%, as previously mentioned. Multiplying CPU efforts of each simulation by their respective parallel efficiency at 32 cores (0.65 for zonal and 0.75 for standard), one obtains 63% of gain using 1 processor. These two values are closely related, with an relative error of less than 2%. It thus validates this method for estimating the computational gains.

One can now use this method to predict the gain of the fine zonal RI simulation over a fine RI simulation. Derivation of the estimated gain is shown in table 5.5(c). Gain is estimated to 66%, with 1 processor, i.e. a speedup of 3.

Zonal algorithm performances

The medium zonal RI simulation requires a global CPU effort of 520 h for a 10 ms simulation. In this CPU duration, the percentages dedicated to GD single grid solver, the ZD single grid solver, the prolongation step, the restriction step and the divergence-free correction step are PRIMARY ATOMIZATION respectively 18%, 62%, 3%, 2% and 15%. Intergrid-communications and correction step thus count for 20% of total CPU effort. The correction step is more costly compare to intergridcommunications since it involves solving implicitly a Poisson equation. Its cost is in the same order than the part relative to GD solver.

The fine zonal RI simulation requires a global CPU effort of 11, 690 h for a 10 ms simulation. In this CPU duration, the percentages dedicated to GD single grid solver, the ZD single grid solver, the prolongation step, the restriction step and the divergence-free correction step are respectively 6%, 82%, 6%, 1% and 5%. Intergrid-communications and correction step thus count for 12% of total CPU effort. This amount is lower than for medium zonal RI simulation since the part relative to ZD solver is higher.

Limitations

In this part, limitations of the current coupling scheme are discussed. 5.17. These velocity oscillations may be thus explained by the non conservation of momentum in the normal interpolation scheme of velocity in prolongation step (see section 3.4.4). The normal interpolation scheme brings variables from cell centroids to face centers. In perspective, other normal interpolation schemes should be tested on a simple test case in order to find out a correct scheme that allows to get rid of these numerical perturbations.

Extending the domain size

In this section, the zonal approach is applied on a geometry of the size of a gas turbine engine combustion chamber. To do so, the current airblast atomizer configuration domain size is extended to the one of an existing combustion chamber. The geometries are derived from [START_REF] Gianluca Motta | Cfd simulation and emissions prediction from a helicopter engine[END_REF]:

The diameter and the length of the combustor are 138 mm and 200 mm respectively, i.e. 111D l and 38D l respectively. Walls are placed on the outer diameter of the combustion chamber as well as around the liquid and gas nozzles (see figure 5 The zonal domain, with medium refinement, is shown in yellow. Its diameter and length are 4D l and 3D l respectively. The global domain, with a very coarse refinement, is shown in black.

refinement will be employed in the zonal domain (see table 5.2) in order to correctly capture the primary and secondary atomization processes: the cell size is around 38 µm between the nozzle exit and x = 3D l . Concerning the global domain mesh refinement, a "very coarse" mesh refinement will be used, detailed there after. With these global and zonal mesh refinements, the refinement ratio between each domain is r x = 4. A zonal simulation will be run with these computational domains and mesh conditions, denominated medium zonal RI extended configuration in table 5.6. RI and TDF models will be used in zonal and global domains respectively, as previously. This very coarse mesh refinement is sufficient after 3D l to capture the largest vortexes, based on a Taylor length scale of 150 µm, calculated a posteriori with the methodology shown in previous part 5.3.2. Similarly, in the farfield near the end of the combustion chamber at x = 110D l , the cell size is set to 1 mm based on the Taylor length scale and some preliminary computations. This very coarse mesh refinement is thus the coarsest refinement allowed for a LES in such configuration.

For comparison of computational costs purpose, a simulation will be run on a few iterations using a single mesh with a medium refinement (medium TDF extended configuration in table 5.6): the cell sizes are set to 38 µm and 1 mm at x = 3D l and x = 110D l , respectively. Thus, the same effective refinements are used at these two locations in both medium zonal RI extended and medium TDF extended configurations (see table 5.6). The TDF two-phase model will be used in this medium TDF extended simulation since it is the one pertinent to use in such a dispersed spray configuration.

Finally, for comparison of qualitative results purpose, a simulation will be run with a single global very coarse mesh along with the TDF model, denominated very coarse TDF extended configuration in table 5 Brown and red text colors stand for very coarse and medium mesh refinements, respectively. RI and TDF models stand for Resolved Interface and Turbulent Diffusive Flux models, respectively.

Qualitative results

The qualitative fields of very coarse TDF extended and the medium zonal RI extended simulations (see table 5.6) are compared in this section.

Three instant shots of the liquid volume fraction are shown in figure 5.20 obtained with the two configurations previously mentioned. The very coarse TDF ext. simulation shows a higher diffusion of the liquid in the ambient air in comparison with the medium zonal RI ext. simulation. Indeed, the correction of the zonal domain with a RI model in the first diameters near the nozzle allows the spray to penetrate further into the combustion chamber.

Performance gains

The computational costs of the medium TDF extended and the medium zonal RI extended simulations (see table 5.6) are compared in this section. The simulations are run in parallel with 12 cores each on the CRIANN super-computer [175] using Myria nodes. Each node is composed of two sockets containing each an 2.4 GHz with 28 cores. Each core offers 128 GB of memory. The nodes are interconnected by Intel Omni-Path Network. Each test is run from t = 0 s to t = 5 × 10 -6 s using adaptive time steps (CFL constraint set up to 0.5). The computational time is evaluated between starting and ending of time loop, to eliminate the influence of initialization routines and I/O during loading of the PRIMARY ATOMIZATION mesh from the storage device. This configuration, with a large main domain and a relative small zonal domain, exhibits the benefits in terms of computational resources saving to use the proposed zonal approach.

Conclusion

In this chapter, it has been shown by means of a coaxial injector simulation that the proposed zonal algorithm is capable of both improving results and reducing the computational cost of a standard finite volume simulation. The idea of the method consists to use two different two phase models in different regions of the computational domain and to refine in time and space the zonal domain.

It has been shown that using a resolved interface model in the whole domain provides results in good agreement with the experiment in the primary atomization region. However, with medium mesh refinement, this model is unadapted upward in the dispersed spray region. Refining the mesh, up to 15 million cells, would lead to a prohibitive computational cost. It is therefore pertinent in this region to keep a moderate refinement and to switch to a subgrid model. That is the purpose of the zonal simulations. Resolved interface model has been used in the zonal domain near the nozzle with two different mesh refinements, medium and fine. In the rest of the domain, a subgrid model has been used with a coarsened mesh to reduce computational cost.

It has been shown that coarsening the mesh in the dispersed spray area allows to save computational resources, up to 58% with medium refinement. In other words, the zonal simulation is 2.4 times faster than a single mesh (standard) one. Scalability tests have been performed prior to the simulations. It has shown good strong scalability speedup and efficiency with the zonal solver, similar to the existing single mesh solvers of OpenFOAM R .

Mass conservation of the zonal approach has also been checked, the liquid volume error is measured to 0.4%, which is in a very acceptable range.

A simulation has been performed with a finer refinement in the primary and secondary atomization region, using the zonal method. Mean liquid core length and mean volume fraction declination along the main axis are closer to experiment data. Performing such simulation with a single fine mesh would have require much more effort, i.e. 2.9 times more CPU hours by estimation (66% of gain).

Chapter 6

Conclusions and perspectives

Conclusions

This PhD thesis has been realized at the CORIA laboratory. It focuses on the development of a coupled multi-domain method applied to two phase flows and primary atomization. The aim is to deal with the multiphysic and multiscale aspects of the atomization process and to reduce the computational cost of such numerical simulations. The purpose of simulating the atomization is to predict the final liquid spray configuration, which is a determinant parameter for the combustion quality in automotive and aeronautic engines among many applications.

A state of the art of the existing multi-domain methods has been performed. The Adapative Mesh Refinement (AMR) methods allow to refine dynamically the mesh with the possibility to use independent blocks refined in time and space, i.e. with a smaller time-step and a smaller cell size than in the underlying block. Among Domain Decomposition Methods (DDM), patched grids use coincident interfaces that allow to have a better conservation of the flow properties between two neighbor zones. DDM methods also give the possibility to resolve various flow models with adapted numerical schemes in each zone. Finally, the zonal grid topology feature allows to keep one global mesh for the overall computational domain and to add when and where necessary embedded refined subgrids.

These four main characteristics have been exploited and implemented in a Two Phase Zonal (TPZ) approach inside the OpenFOAM R library. The two important features of this approach are (i) the refining in time and space of an independent zonal domain and (ii) the possibility to use different two-phase models: A resolved interface model that captures the liquid-gas interface, here Volume Of Fluids (VOF) model, and a diffuse interface model that follow the interface density with sub-grid terms, here ELSA (Euler Lagrangian model for Spray and Atomization) model. The emplacement and size of the zonal domain is set-up by the user prior to the simulation. The boundaries should be placed in zones with relatively calm flow features, i.e. low velocity and volume fraction gradients.

This coupled approach has been validated on two simple test cases, a rising bubble problem and a liquid-air jet . In both cases, the results obtained with a refined zone and a coarse mesh are in good agreement with those obtained with a full refined mesh. The speedup of the zonal approach is in a range of 1.7 to 3.7, depending on the mesh sizes and refinements. Several parameter studies have been performed in order to assess the influence of each parameter and scheme in the zonal solver.

The zonal solver has also been parallelized in order to apply it on an atomization process. The parallelization developments aim to distribute the data between processors for the inter-grid interpolation processes.

An additional development has consisted to extend this zonal approach to the coupling of a Lagrangian Smoothed Particle Hydrodynamics (SPH) solver with a Finite Volume (FV) solver.

The Lagrangian solver employs a weakly compressible SPH method, which is efficient when dealing with two phase interfaces and convective problems. The FV solver uses an incompressible solver. The SPH method has been implemented in the OpenFOAM R library and validated over several test cases including a Poiseuille flow and a plane jet in a coflow. Then, it has been coupled with Finite Volume with the aim to reduce the diffusion of a transported passive scalar in the latter domain. The results show a satisfying correction when the jet is covered by the SPH domain. The coupling scheme between these compressible and incompressible methods should be improved and the computational cost of the SPH method should be reduced in order to apply this coupling on more complex configurations.

Finally, the parallelized finite volume TPZ approach has been applied on a coaxial atomization configuration. The zonal domain is placed near the nozzle injector and extended up to 3 diameters further. Inside this domain, the resolved interface model allows to capture well the liquid core penetration given by experimental results. Downstream the zonal domain boundary, the diffuse interface model manages to resolve the dispersed two phase flow topology with a coarse mesh refinement. This brings a speedup in comparison with a standard and single model solver up to 2.7. When extending the geometry to the size of a combustion chamber, the speedup is increased to 33.

Perspectives

Perspectives of developments and applications for this zonal methodology are numerous. Let's mention some of them:

• In the simulations shown in this work, coupling between zonal and global domains was operational during the whole run, from initial to final instants. Initial conditions were set up in pre-processing for both domains. Depending on the configuration, in order to save computational resources, this coupling could be activated only when necessary in the simulation. It would start with the global coarse domain only, until a user-defined time from which starts the coupling with a fine zonal domain. To initialize the zonal conditions, mapping of solution between meshes will be necessary. The procedure for interpolating coarse global field to zonal mesh has been treated in section 3.4.7.

As example, in the airblast atomizer configuration, a coarse simulation can be run first without the zonal correction until the initial transient state is over. Then, the zonal fields are initialized with a suitable mapping process and the zonal coupled simulation is started.

An example of application is solitary breaking wave propagation. In coastal and ocean engineering, accurate simulations of water waves [START_REF] Tonelli | Finite volume scheme for the solution of 2d extended boussinesq equations in the surf zone[END_REF][START_REF] Kazolea | An unstructured finite volume numerical scheme for extended 2d boussinesq-type equations[END_REF][START_REF] Kazolea | Numerical treatment of wave breaking on unstructured finite volume approximations for extended boussinesq-type equations[END_REF] in realistic environments are important and have largely replaced laboratory experiments for the design of coastal structures. Simulation of such flows involves wave propagation during a relatively important period of time before occurs the impact with solid. During this time lapse, it is not necessary to obtain an accurate solution near the solid, hence to have a fine mesh in this area. An application of our zonal methodology would thus consist to run the simulation with a single coarse mesh during the solitary wave propagation and then to start the zonal coupling with a finer zonal mesh when the wave is near the solid. Illustration of such a configuration is shown in figure 6.1.

• A single-phase application example of the zonal approach would be computational aerodynamic flow around an airfoil. Mesh refinement efforts have to be focused around the airfoil in order to obtain accurate drag and lift forces estimations. At the same time, the computational domain has to be relatively large in comparison with the airfoil size to avoid any block effects. A refined zone could be thus employed near the airfoil coupled with a coarser large domain without impacting the computational time-step. This method is similar to overlapping block methods, at the difference that subcycling in time between two block is used.

• The current developments take in account a single zonal domain coupled with a global domain. Further developments should allow to simulate several zonal domains coupled with the same global domain. Multi-injection inside a annular combustion chamber is an example of application. In gas turbines, most chambers use multiples sectors, from 15 to 24 typically, each one of them being fed by its own fuel injection system. In order to study the flame propagation from sector to sector and the azimuthal instability modes, a simulation of the whole chamber is necessary [START_REF] Wolf | Using les to study reacting flows and instabilities in annular combustion chambers[END_REF]. LES of such domains remain very costly or can even be out of reach. The utilization of a zonal domain for each injector could allow to reduce the computational efforts, by refining only near each injector. Furthermore, switching between different models is pertinent in such multiphysic configuration, involving atomization and combustion.

• The coupled solver currently handle two levels: a coarse global domain and a finer zonal one, with a refinement ratio r > 2. In perspective, several layers of domains with successive higher levels could be handled in the solver. It will allow to manage successive regions at different time and space scales.

• In the current finite volume zonal approach, there is room to improve the momentum and free stream conservation aspects of the coupling procedure. The time sub-cycled AMR algorithms developed by [START_REF] Ann S Almgren | A conservative adaptive projection method for the variable density incompressible navierstokes equations[END_REF][START_REF] Daniel | A cell-centered adaptive projection method for the incompressible euler equations[END_REF]1] provide possible solutions. To improve the momentum conservation at the coarse-fine interface, a refluxing correction of velocity values in coarse cell centers along the interface could be performed after the restriction step [START_REF] Daniel | A cell-centered adaptive projection method for the incompressible euler equations[END_REF]1]. In the divergence free correction step, the Poisson equation should be solved simultaneously in both zonal and global domains in order to obtain consistent face flux fields [1]. It is currently solved only in global domain, after the restriction step.

Another point of improvement is the interpolation procedure from the global coarse domain the zonal fine domain. Currently, prior to the resolution of the zonal domain solution, only coupled boundary conditions are updated based on an interpolation process in time and space. In order to reduce the computational cost of resolution of the zonal domain solution, the full zonal domain could be updated based on an interpolation process in time and space. This interpolation would be similar to the prolongation of a full solution in a Full Multigrid cycle (see part 2.12). This interpolation can be a first approximation of the sought solution and thus reduce the required number of iterations to converge.

At last, the free stream preservation [START_REF] Ann S Almgren | A conservative adaptive projection method for the variable density incompressible navierstokes equations[END_REF][START_REF] Daniel | A cell-centered adaptive projection method for the incompressible euler equations[END_REF]1] could be included in the current coupling scheme. See section 3.2.1.2 for more details about the free stream preservation.

• A demonstration of coupling between Weakly Compressible Smoothed Particle Hydrodynamics (SPH) solver and an incompressible Finite Volume (FV) solver has been shown in this thesis. There is room to improve (i) the computational performances of the SPH solver and (ii) the coupling scheme.

(i) The KIT developements [START_REF] Braun | Modeling fuel injection in gas turbines using the meshless smoothed particle hydrodynamics method[END_REF][START_REF] Braun | Hpc predictions of primary atomization with sph: Challenges and lessons learned[END_REF][START_REF] Koch | Prediction of primary atomization using smoothed particle hydrodynamics[END_REF] show that the SPH method is able to simulate complex two-phase flow configurations and a primary atomization process with a reasonable computational cost. As an example of serial optimization of the SPH algorithm, the structure of arrays data layout is more efficient than the array of structures: instead of storing the particle attributes in a list of particle structures, they are stored in separate arrays. Thus, when performing calculations on the data, only the required data of the particles under concern is loaded. The caches have to be refreshed much less frequently.

(ii) The coupling between a compressible SPH solver and an incompressible Finite Volume solver should then be improved by means of an active correction of the finite volume fields (velocity, face fluxes and pressure) after the restriction step. Generation of particles at the coupled boundaries should also be performed in the future to take in account mass entry. The work of Kassiotis et al. [START_REF] Kassiotis | Semi-analytical conditions for open boundaries in smoothed particle hydrodynamics[END_REF] provides a possible solution.

• In the current employed sub-grid two-phase model, effects of evaporation are not taken in account. Thus, spray evaporation can be taken in account into the model by including an additional transport equation for vapor fuel fraction and an appropriate sink term in the transport equation for liquid fuel fraction.

• Finally, the current number of processors per domain (zonal and global) is currently equal. It is not optimized for meshes with different orders of size. As a perspective of development, the number of processors should be specific to each domain. ALGORITHM this GD sub-domain bounding box ?

• 3 rd step (stages 3 to 5 in algorithm) consists to distribute data between processors. Data that are distributed are all incomplete donors/acceptor pairs (with only acceptor information) that have been stored in first step and acceptor relative informations that are face normals, face areas and cell bounding box.

• 4 th step (stage 6 in algorithm) consists to associate donors and acceptors. The criteria is: Which donor face center is the closest to this acceptor patch face center ? When an eligible donor is found (there must be one), its index is then check to know if it is an internal face or a patch face. Since number of internal faces in GD is known, it is a patch face if its index is higher than this previous number. Indeed, index here is the primitive mesh index, where no distinction is made between internal and patch faces yet. But we aim to store the patch face index for later. If it is a patch face, it means this a processor patch since physical boundaries in GD are not coupled with ZD. In that particular case, a loop is made over GD patches to find the patch index and the patch face index. Finally, all necessary informations relative to the donor are known and are now stored: the finite volume face index (internal index or patch index), the processor number, the face center coordinates, the patch index (if it is an internal face, a hard-coded value -1 is stored) and the coordinates of the surface vector.

• 5 th step (stages 7 to 10 in algorithm) consists to distribute data between processors. Data that are distributed are all donors/acceptor pairs that have been established in previous step.

• 6 th step (stage 11 in algorithm) consists to treat duplicates. Duplicates are two donors/acceptor pairs with same acceptor index. In case of a duplicate, selection is made on least distance from acceptor face center to donor face center. The pair with least distance is kept while the other one is deleted.

A.2 Cell center restriction

The acceptor cells are located in Global Domain, more precisely in the covered part. This covered part is a region defined by the user in preprocessing for generating Zonal Domain mesh. Thus, number of acceptor cells is already known, in each GD sub-domain (processor), as well as number of donor cells in each ZD sub-domain.

A cell center restriction consists of volume averaging all fine donor cells overlying one coarse acceptor cell. Thus, one acceptor cell is associated with one or more donor cells.

The different step of the algorithms are detailed below, with even more details in the second appendix B in which the code algorithm is also reported.

• 1 st step (stage 1 in algorithm) consists to store acceptor informations: index, processor number and location coordinates. It is not necessary to store their types since acceptors are only internal field cells. Extra geometry data about acceptor cell are also stored, that will be needed for establishing donor/acceptor pair. These extra data are centers and A.2 Cell center restriction 219 normals of each face composing this acceptor cell and the cell bounding box. With these three data, one can known later if a donor centroid is inside the acceptor cell or not.

• 2 nd step (stage 2 in algorithm) consists, for each processor, to known the number of acceptors to send to other processors. The criteria is: Does this acceptor cell bounding box overlap this ZD processor domain bounding box ? Two bounding boxes, BB 1 and BB 2 , are overlapping each other if following statement is true:

x max (BB 1 ) > x min (BB 2 ) , x min (BB 1 ) < x max (BB 2 ) , (A.1) where x min (BB i ) and x max (BB i ) are respectively the minimum and maximum coordinates of bounding box BB i .

• 3 rd step (stages 3 to 5 in algorithm) consists to distribute data between processors. Data that are distributed are all incomplete donors/acceptor pairs (with only acceptor information) that have been stored in first step and acceptor relative informations that are face normals, face areas and cell bounding box.

• 4 th step (stage 6 in algorithm) consists to associate donors and acceptors. The criteria is: Is this donor cell centroid is inside this acceptor cell ? In mathematical formalism, a donor cell centroid is inside an acceptor cell if the following statement is true:

n f • (P -C f ) ≤ 0 ∀f , (A.2)
where f denotes each face of the acceptor cell, n f is the face normal, C f is the face center and P is the donor centroid. Two examples are given in figure A.1 with an arbitrary acceptor cell shape. In first example (a), donor cell centroid is inside the acceptor cell and all scalar products between face normals n and face distances d are negative. In second example (b), donor cell centroid is not inside the acceptor cell since at least on scalar product is positive. This test (A.2) is only valid for plane faces.

When a cell donor candidate is valid, i.e. inside acceptor cell, relative informations are stored: its local index, its processor number, its location coordinates and its cell volume, the former one will be used for volume averaging in interpolation step.

In order to limit the number of donor candidates, a pre-selection is made by using acceptor cell bounding box. A donor candidate is a cell whose centroid is inside acceptor bounding box, i.e. between its minimum and maximum coordinates.

• 5 th step (stages 7 to 10 in algorithm) consists to distribute data between processors. Data that are distributed are all donors/acceptor pairs that have been established in previous step.

• 6 th step (stage 11 in algorithm) consists to treat duplicates. Duplicates are two donors/acceptor pairs with same acceptor index. This particular case occurs when one acceptor bounding box is overlapping several ZD sub-domains. In case of a duplicate, one pair receives all donors of the other pair. Then, this last one is deleted. ALGORITHM P . In (a), point is inside and all scalar products between face normals n and face distances d are negative. In (b), point is outside and two scalar products are positive.

A.3 Face center restriction

The acceptor faces are located in Global Domain, more precisely in the covered part. This covered part is a region defined by the user in preprocessing for generating Zonal Domain mesh. Numbers of acceptor faces and donor faces are not known before starting the algorithm.

A face center restriction consists of surface averaging all fine face cells overlying one coarse acceptor face. In case of flux interpolation, it consist of summing all fine fluxes to obtain the corresponding coarse flux. Thus, one acceptor face is associated with one or more donor faces.

To avoid parallelization errors and to easier the programming, the distribution algorithm for cell center restriction will be used. The idea is to store informations relative to faces inside their owner cell and distribute these informations with the cell center restriction algorithm, previously detailed. Donors/acceptors association algorithm can be synthesized in three steps:

• 1 st step (stage 1 in algorithm) consists to find out all eligible face donors and to "pack" it in their respective owners.

• 2 nd step (stage 2 in algorithm) consists to distribute packed data by using the cell center restriction algorithm.

• 3 rd step (stage 3 in algorithm) consists to "unpack" eligible faces donors and associate it with an acceptor face.

1 st step and 3 rd step processes are described below.

It is important to note that not all faces in ZD are eligible donor faces. Indeed, only coincident faces between ZD and GD will be associated. It corresponds to configurations (a), (c), (e) and (g) in figure A.2.

A.3.1 Packing process

The packing process converts face informations into cell informations. Only hexahedral elements are considered in current developments. We thus assume that each donor cell will stock at maximum:

• 3 faces for a ZD/GD refinement ratio r x > 1. This case occurs, in three dimensions, when a donor cell is located in the corner of an acceptor cell (example: configuration (a) in figure A.2).

• 6 faces for a ZD/GD refinement ratio r x = 1. This case occurs, in three dimensions, when a donor cell owns all faces that compose itself, i.e. its 6 faces.

The previous assumption about possible maximal values will be an efficient way to test that everything went fine in the packing process. At the end of the process, the number of faces stocked in each cell will be checked. To find out all eligible faces donors and pack it in their respective owner cells, two loops are performed: one over all ZD internal faces, then one over all ZD patch faces. If f Z is an eligible donor, then the following informations are stored in its owner cell P Z : donor face index, donor type (here internal face), index of GD neighbor N G (for finding back global face later), donor face center coordinates and donor face normal vector coordinates. A particular case occurs when the respective processors of P G and N G are not the same (configuration (e) in figure A.2). It means that acceptor face f G is a patch face, between two processors. It is thus necessary to stock donor face f Z informations both in owner cell f Z and neighbor cell N Z . In that way, each patch f G located on two different processors will receive the informations relative to the donor face.

• Then, a second loop is performed over all ZD patch faces. Illustrations of possible configurations are shown in subfigures (c), (d), (g) and (h) in figure A.2. Two possibilities arise concerning patch face f Z :

-Patch face f Z is a processor patch face. In that case, to known if it is an eligible donor or not, one computes a virtual neighbor cell center to see if it is inside or not ALGORITHM

P Z . N Z . f Z P G . N G . f G (a) P Z . N Z . f Z P G . N G . f G (b) P Z .
f Z (patch)

P G . N G . f G (c) P Z .
f Z (patch)

P G . N G . f G (d) P Z . N Z . f Z P G .
f G (patch) (e)

P Z . N Z . f Z P G .
f G (patch) (f) where β is hard-coded value equal to 0.1. This virtual cell center N virt,d is inside acceptor cell P G if the statement (A.2) is true. If f Z is an eligible donor, its relative informations are stocked inside its owner cell. Donor type specified here is processor patch face. It is to note that the same face will thus be sent to the same acceptor by the neighbor processor (on the other side of the patch). Thus, interpolated value will be divided by two later to take in account this particular case.

P Z . f Z (patch) P G . f G (patch) (g) P Z . f Z (patch) P G . f G (patch) (h)
-Patch face f Z is a either a boundary condition patch face either a ZD/GD interface patch face. It is thus an eligible donor. Indeed, the fluxes may not be consistent at the boundary conditions and at the interface since time refinement, space refinement and solvers are different. Thus, it is highly preferable that face restriction is effectuated also along all ZD patch faces. It will correct GD boundary condition values and GD internal values along the ZD/GD interface. Concerning the interface topology, it is properly placed, faces between ZD and GD are coincident (see subfigure (c) in figure A.2). Concerning the ZD boundary conditions, they are superimposed with GD boundary conditions (see subfigure (g) in figure A.2). Thus, all patch faces f Z (except processor patch) are eligible donors.

Finally, after the two previous loops over internal and patch faces, a test is realize to check if the maximum number of faces stocked in each ZD cell is not higher than the maximum allowed (3 faces for a ZD/GD refinement ratio r x > 1, 6 otherwise).

A.3.2 Unpacking process

After packed informations have been distributed between processors, it is now necessary to find out all acceptor faces and associate it with donors. A loop over all restriction acceptor cells in GD is performed. For each acceptor cell, a loop is performed over all its restriction ZD donor cells, and finally, for each donor cell, a loop is performed over all its packed eligible donor faces.

First step to deal with is the case where acceptor neighbor cell N G is unknown. It can be because either donor face is a patch face either acceptor face is a patch face. In the first case the neighbor can be found, while in the second it can not. Thus, let us try to find the neighbor cell by means of a a virtual neighbor cell center N virt whose position is calculated with relation (A.3). It is then checked in each neighbor cells of the acceptor cell P G if N virt if the virtual cell center is inside (with relation (A.2)). If it is inside one of the neighbor cells, then it means that acceptor face f G is an internal face. Index of the neighbor acceptor cell is stored. Labels inside sending map rectangles are element indexes (cell, face,...) being sent to other processors. Labels inside received map rectangles are constructed indexes, i.e. indexes offset by the number of values received by previous processors. These two maps are input data for a mapDistribute object that allows to distribute data (index by the same elements) between processors.

When sending and received maps are assembled, a distributing map can be constructed. It allows to easily distribute any data (scalar, vectors, etc...) , indexed with same elements used in sending map, between all the processors.

φ

  field variable (pressure, velocity or density) -ρ density M.L -3 kg m -3 τ stress tensor M.L -1 .T -2 Pa

  . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4.10 State-of-the-art chronology of SPH-FV coupling . . . . . . . . . . . . . . . . . . 4.11 SPH domain in Kumar's SPH-FV coupling method. . . . . . . . . . . . . . . . . 4.12 Finite volume-SPH zonal coupling algorithm. . . . . . . . . . . . . . . . . . . . . 4.13 Configuration of Global Domain (GD) and Zonal Domain (ZD) for a plane jet in a coflow following Aristodemo et al. configuration [4]. . . . . . . . . . . . . . . . 4.14 Passive scalar γ field at tU/D = 6 for three different resolutions in Finite Volume. 4.15 Passive scalar γ fields at different times, without zonal SPH correction (left, figures (1)) and with zonal SPH correction (right, figures (2)). . . . . . . . . . . . 5.1 Schematic of the injector used by Stepowski et al. [5]. . . . . . . . . . . . . . . . 5.2 Dimensions and boundary conditions of the computational domain. . . . . . . . . 5.3 Liquid inlet patch faces for three different mesh refinement. . . . . . . . . . . . . 5.4 Evolution of computed mean gas flux divided by mean gas flow rate, in both domains of the zonal simulation. . . . . . . . . . . . . . . . . . . . . . . . . . . .

Figure 1 . 1 :

 11 Figure 1.1: Example of early utilization of atomization process by humans: rock painting. Here, several negative hand prints in the cave of Cueva de las manos in Argentina.

Figure 1 . 2 :

 12 Figure 1.2: Schematic representation of physical processes occurring inside a combustion system, here an automotive combustion chamber with pressure atomizer.

Figure 1 . 3 :

 13 Figure 1.3: Atomization process scheme.

Figure 1 . 4 :

 14 Figure 1.4: Four modeling approaches for two-phase flow.

(

  a) Euler-Lagrange model; (b) an Euler-Euler method: two-fluid model; (c) a single-fluid and Eulerian method: Volume of Fluid (VOF) method; (d) a single-fluid and Lagrangian method: Smoothed Particle Hydrodynamics (SPH) method.

Figure 2 . 2 :

 22 Figure 2.2: Vectors d and S on an orthogonal mesh.

Figure 2 . 3 :

 23 Figure 2.3: Non-orthogonality treatment in the "minimum correction" approach.

Figure 2 . 4 :Figure 2 . 5 :

 2425 Figure 2.4: Non-orthogonality treatment in the "orthogonal correction" approach.

Figure 2 . 6 :

 26 Figure 2.6: Control volume with a boundary face.

. 72 )-

 72 Diffusion term: The dot product between the face area vector and (∇φ) b is known to be S • (∇φ) b = |S|g b , (2.73) and the resulting diffusion term is: Γ b |S|g b .

( 6 )( 7 )

 67 If pressure is not imposed on boundaries, adjustment of computational domain outflow (5) Solve implictly pressure gradient ∇p m = f (∇p m , F ) Add pressure gradient to velocity U m = f ( Ũ , ∇p m ) Add pressure gradient to face flux

Figure 2 . 10 :

 210 Figure 2.10: Vectors d and S on a non-orthogonal face with a 27 • deviation.

Figure 2 . 11 :

 211 Figure 2.11: Vectors d, S and δ i on a skewed face.

Figure 3 . 1 :

 31 Figure 3.1: Three types of AMR methods.

( a )

 a Original coarse grid with tagged cells for refinement. Applied refinement with (b) Cell-based method, (c) Patch-based method and (d) Block-based method.

Figure 3 . 2 :

 32 Figure 3.2: Block-based time-subcycled AMR algorithm of Martin et al. [1], for two levels of refinement.

Figure 3 . 3 :

 33 Figure 3.3: Possibility of arrangements for two independent grids in DDM techniques.

Figure 3 . 4 :

 34 Figure 3.4: Configuration of a zonal embedded grid in a turbulent channel flow.

Figure from [ 107

 107 Figure from[START_REF] Manhart | A zonal grid algorithm for {DNS} of turbulent boundary layers[END_REF].

Figure 3 . 5 :

 35 Figure 3.5: The face f whose owner is cell center P and neighbour cell center N .

  .27) with subcycle index i ∈ [1, N αSC ] and subcycle time-step δt = ∆t/N αSC . The initial α i is initialized with α i = α n . At the end of the loop, α n+1 = α i+1 . Depending on the solver, equation 3.23 or 3.26 is used to recursively determine F α in equation 3.27.

. 29 )( 2 )

 292 (TDF) Transport equation of α with Turbulent diffusive flux term of equation 3.24 is now determined. We introduce α D,adv as previous solution of advective transport equation 3.27:

( 5 . 2 )

 52 Computing pseudo-volumetric face flux:A pseudo-volumetric face flux is computed based on pseudo-velocity Ũ interpolated to face f . Fu = Ũ f • S .(3.40)

. 41 )( 5 . 3 ) 4 )

 41534 Implicit pressure direct solution:Poisson equation for pressure is implicitly solved for computing pressure at iteration index m, Volumetric face flux corrector: Contribution of pressure term is added to volumetric face flux,

( 6 )

 6 Solve additional transport equations. (5.1) Compute pseudo-velocity Ũ . (5.2) Compute pseudo-face flux F . (5.3) Implicitly solve pressure P rgh . (5.4) Compute face flux F . (5.5) Compute velocity U . (5.6) Go back to (5.1) or update solution at index n + 1..

Figure 3 . 6 :( 6 )

 366 Figure 3.6: Algorithm structure of both single grid two-phase solvers.

3 /Figure 3 . 7 :

 337 Figure 3.7: Global and zonal domains.

( 4 )

 4 Correction of GD solution: 1) A Poisson equation is solved to correct volumetric face flux field. 2) Volume fraction values in cells along the ZD interface (lying outside) are corrected. 3) Mixture properties are updated.

Figure 3 . 8 :

 38 Figure 3.8: Zonal methodology algorithm.

  .55) Equation (3.55) is resolved iteratively starting from last known value. -(TDF) An explicit expression for face center phase indicator field is derived from equations (3.28) and (3.31):

Figure 3 . 9 :

 39 Figure 3.9: Interface Γ between Zonal Domain (ZD) and Global Domain (GD) for a mesh resolution ratio r x of 2:1.

Figure 3 . 10 :

 310 Figure 3.10: Three types of interpolation between Zonal Domain and Global Domain.

  (a) Face-to-patch prolongation; (b) Cell center restriction; (c) Face center restriction. Zonal domain and global domain are shown in red and blue, respectively. The mesh refinement is r x = 2.

1 ΓFigure 3 . 11 :

 1311 Figure 3.11: Simulation domain, boundary conditions and initial configuration of Hysing et al. [2] rising bubble problem.

3. 5 Validation of the strategy 97 Configurations 3 :

 5973 Main (global) domain Zonal domain Mesh ref. Mesh size Two-phase model Mesh ref. Mesh size Two-phase model Coarse Two-phase numerical simulations performed in the rising bubble configuration.

Figure 3 . 13 :

 313 Figure 3.13: Evolution of bubble rising velocity.

Figure 3 . 14 :Liquid density ρ 1 Gas density ρ 2

 31412 Figure 3.14: Configuration of the liquid-air jet configuration. The zonal domain (ZD), with fine refinement, is shown in yellow. Main (global) domain (GD), with coarse refinement, is shown in black. Γ stands for the zonal domain interface with global domain and is shown with yellow line. Liquid injection Turbulent intensity T i Turbulent length scale l Velocity U 1 Injector diameter D 7.5 % 10 µm 100 m/s 100 µm Property Surface tension σ Liquid density ρ 1 Gas density ρ 2 Liquid viscosity µ 1 0.07 kgs -2696 kgm -3 25 kgm -3 6.96×10 -4 kg m -1 s -1

Figure 3 . 15 :

 315 Figure 3.15: Zoom on the fine zonal mesh near interface. The zonal domain (ZD), with fine refinement, is shown in yellow. Main (global) domain (GD), with coarse refinement, is shown in black. The fine mesh refinement relative to the coarse refinement is 5 : 1 in the y-direction close to the jet center line and 2 : 1 otherwise.

. 19 .Figure 3 . 16 :Figure 3 . 17 :Figure 3 . 18 :

 19316317318 Figure 3.16: Transient state liquid volume fraction fields obtained with two zonal runs. The transient time is at tU/D = 13. The fields are obtained using (a) TDF solver and (b) RI solver in both domains. The zonal interface Γ is shown with white lines.

  Volume fraction field obtained in transient state with the RI zonal simulation is shown in figure3.16-(b). The jet tip is numerically diffused by the coarse mesh refinement when crossing the interface Γ. Volume fraction and velocity fields obtained in steady state with the zonal simulation are shown in figure3.21. The liquid jet penetrates further. It means that liquid volume fraction does not diffuse, compared to the TDF model field (figure3.17-(a)). Indeed, RI model requires a finer mesh and a three dimensional computation among other characteristics to capture the atomization process. The velocity gradient between the liquid jet and the gas are stronger in this configuration than with TDF model (figure3.17-(b)).

Figure 3 . 19 :

 319 Figure 3.19: TDF model: Velocity and liquid volume fraction profiles along jet center line. Velocity and liquid volume fraction profiles are respectively in left and right parts. Three different instants are shown: (a) tU D = 5; (b) tU D = 15; (c) tU D = 85. Zonal domain interface Γ at x = 11D is indicated by a vertical dashed line.

Figure 3 .Figure 3 . 21 :Figure 3 . 22 :

 3321322 Figure 3.20: TDF model: Evolution of volume of liquid using the zonal grid solver.

  RI and TDF solvers are used in zonal and global domains respectively. During the prolongation step, TDF phase fraction α D is used to obtain boundary conditions for RI phase fraction α I at the zonal interface. Then, during the restriction step, RI phase fraction α I allows to correct the TDF field in the covered region of GD. Steady state volume fraction and velocity fields are shown in figure 3.24. Diffusion of the liquid occurs later, after 11 diameters, i.e. the interface Γ, compared to the TDF model field in figure 3.17-(a). Steady state phase fraction and velocity profiles obtained with such hybrid simulation are shown in figure 3.25. TDF model diffusion starts after the interface Γ as shown in figure 3.25-(b). Upstream, the flow is governed by RI model in the covered region. This hybrid profile is bounded by RI and TDF fine profiles. Velocity profile matches reference fine RI profile in the zonal region. Downstream the zonal interface, it converges with TDF profile. The transition between the two models is smooth thanks to the Neumann boundary condition at Γ.

Figure 3 . 23 :Figure 3 . 24 :Figure 3 . 25 :

 323324325 Figure 3.23: RI model: Velocity and volume fraction profiles along jet center line.Velocity and liquid volume fraction profiles are respectively in left and right parts. Three different instants are shown: (a) tU D = 5; (b) tU D = 15; (c) tU D = 85. Zonal domain interface Γ at x = 11D is indicated by a vertical dashed line.

  Schemes

Figure 3 . 26 :

 326 Figure 3.26: Evolution of bubble rising velocity for two different face interpolation schemes of phase indicator.Scale is zoomed on velocity peaks.

Figure 3 . 27 :

 327 Figure 3.27: Temporal evolution of relative mass error in rising bubble test case for two different face interpolation schemes of phase indicator.

Figure 3 . 28 :

 328 Figure 3.28: Evolution of bubble rising velocity for different interpolation schemes in time with refinement r x = 2.

Figure 3 . 29 :

 329 Figure 3.29: Evolution of bubble rising velocity for different tangential interpolation schemes with refinement r x = 2.

  (injection) Coarse + ZD (linear) Coarse + ZD (skewed linear) (b) -tU D = 85 Figure 3.30: RI model: Velocity profile along jet center line for different tangential interpolation schemes.Zonal Domain interface at x = 11D is indicated by a vertical dashed line.

85 Figure 3 . 31 :

 85331 figures 3.30 for RI model and in figures 3.31 for TDF model.

Figure 3 . 32 :

 332 Figure 3.32: Evolution of bubble rising velocity using either coupled gradient either zero gradient for coupled inlet-outlet boundary condition in zonal grid.

Figure 3 . 33 :

 333 Figure 3.33: Temporal evolution of cumulated clipped mass in the liquid-air jet configuration.

Figure 3 . 34 :

 334 Figure 3.34: Mass error evolution in bubble rising configuration using either coupled gradient either zero gradient for coupled inlet-outlet boundary condition in zonal grid.

85 Figure 3 . 35 :

 85335 RI model: Velocity profile along jet center line, using either Dirichlet either inletoutlet coupled boundary condition for velocity in zonal grid.

  (a) a coupled Dirichlet condition is used for velocity with a Neumann condition for pressure (equation 3.62), (b) a mixed Dirichet/Neumann condition (inlet-outlet) is used for velocity with a coupled Dirichlet condition for pressure.

Figure 3 . 36 :

 336 Figure 3.36: Evolution of bubble rising velocity with three different types of coupled boundary conditions for velocity in zonal grid.Dirichlet U stands for full coupled Dirichlet conditions; inlet-outlet U stands for full coupled inlet-outlet conditions; semi inlet-outlet U stands for coupled Dirichlet on the lower side interface and coupled inlet-outlet on the rest of the interface.

Figure 3 .

 3 Figure 3.35 shows the steady state velocity profile along symmetry axis in the liquid-air jet configuration, using RI model. The profile obtained with the conditions (a) is not bounded between coarse and fine profiles. Indeed, when leaving the region covered by ZD, the flow is faster than expected. It can be explained by the flux directions at the upper ZD/GD interface that are not respected, because of the Dirichlet constraint on velocity. In this configuration, where most of the information transfer is one-way, i.e. leaving ZD and going into GD, conditions (b) (Dirichlet for pressure and inlet-outlet for velocity) are more appropriated. The profile obtained with conditions (b) is well bounded between coarse and fine profiles.

Figure 3 .

 3 Figure 3.36 shows bubble rising velocity with the two combinations plus a third one (c), detailed later. In this configuration, the conditions (a) show good results, close to fine and coarse profiles, while conditions (b) are severely unbounded and far from expected profile. Two explanations arise concerning these last results: First, in this bubble configuration, using conditions (b), ZD boundary conditions for pressure are fully Dirichlet. The boundaries of the Poisson equation are thus over-constrained. Second, the flux mismatch for velocity is not corrected in coarse cells along coarse-fine interface Γ. A correction similar to the phase flux correction step should thus be performed after the restriction step.

85 Figure 3 . 37 :

 85337 RI model: Velocity profile along jet center line for three different zonal domain sizes.Zonal domain interfaces of short domain (x = 5.5D), medium domain (x = 11D) and long domain (x = 16.5D) are indicated by vertical dashed lines respectively in red, blue and green colors.

Figure 3 .

 3 Figure 3.38: RI model: Velocity relative difference in each cell between two domains, with coarse refinement.

( a )Figure 3 . 39 :

 a339 Figure 3.39: Simulation domain of Hysing et al. [2] rising bubble problem with different size and placements of zonal domain. Interfaces Γ of high, low and tall zonal domains are respectively shown in red, blue and orange.

Figure 3 .Figure 3 . 40 :

 3340 Figure 3.38 shows velocity relative difference fields with these three ZD lengths. Difference is highly reduced whatever the sizes of the zonal domain. A high difference spot appears on

Figure 3 . 41 :

 341 Figure 3.41: Temporal evolution of relative mass error in rising bubble test case, with and without phase indicator correction along interface Γ.

. 97 )

 97 where |U old rec | is the magnitude of the reconstructed velocity before face flux correction. Relative variation fields in jet configuration are shown in figure 3.42, for four different times. Interface of Zonal Domain Γ is shown in yellow. RI model has been used in this simulation.

  (a) -tU/D = 10. (b) -tU/D = 15. (c) -tU/D = 25. (d) -tU/D = 85.

Figure 3 . 42 : 128 CHAPTER 3 .Figure 3 . 43 :

 3421283343 Figure 3.42: Relative difference of cell center face flux before and after face flux correction step. Zonal Domain interface Γ is shown in yellow.

  (divergence free correction) Coarse + ZD (no correction)

Figure 3 . 44 :

 344 Figure 3.44: RI model: Velocity profile along jet center line, with and without divergence free correction procedure. Zonal Domain interface at x = 11D is indicated by a vertical dashed line.

Figure 3 . 45 :

 345 Figure 3.45: Possibilities of processor arrangements in Global Domain and Zonal Domain, here with 4 processors. The labels stand for the processor number. (a) Unified decomposition ; (b) Equivalent decompositions ; (c) Optimized decompositions. The configuration considered for the solver parallelization is (b).

Figure 3 . 46 :

 346 Figure 3.46: Example of strong speed-up profile for a parallelized solver.

Figure 3 . 47 :

 347 Figure 3.47: Parts of the zonal methodology algorithm that have been parallelized. See figure 3.8 for more details about the notations. Parts of the algorithm that need parallelization are circled with dashed orange rectangles, while parts already parallelized in OpenFOAM R library are shaded.

Figure 3 . 48 :

 348 Figure 3.48: Liquid-gas interface at t = 3 s of Hysing skirted bubble configuration [2] obtained with zonal simulations using a different number of processors.

Figure 3 . 49 :

 349 Figure 3.49: Evolution of bubble rising velocity obtained with zonal simulations using a different number of processors.

Figure 4 . 1 :

 41 Figure 4.1: Eulerian and Lagrangian representation of fluid flow equation. Figure from [3].

W

  (xx , h) dx = 1 . (4.29) (ii) Delta function property:

Figure 4 . 2 :

 42 Figure 4.2: Illustration of wall modeling by using ghost particles.

4.2 Smoothed Particle Hydrodynamics 153 4. 2 . 4 . 8

 153248 Improvement of the accuracy of the Kernel-based approximation

Figure 4 . 3 :

 43 Figure 4.3: Comparison of velocity profiles for a low Reynolds Poiseuille flow obtained with a Weakly Compressible SPH simulation and an analytical solution.

Figure 4 . 4 :

 44 Figure 4.4: SPH velocity field obtained on the low Reynolds Poiseuille flow configuration.

Figure 4 . 5 :

 45 Figure 4.5: Laminar jet in a coflowing environment

  Equation system: Mass conservation: equation 4.42. Momentum conservation: equation 4.47.

4. 3

 3 Validations 159 Equation of motion: equation 4.48. State's equation for pressure: equation 4.49.

33 Figure 4 . 6 :

 3346 Evolution of the phase field in a laminar jet in a coflow configuration, obtained with Weakly Compressible SPH.

  Black and grey particles stand respectively for jet and coflow particles.

Figure 4 . 7 :

 47 Evolution of the phase field in a laminar jet in a coflow configuration, obtained with an incompressible finite volume solver.

Figure 4 . 8 :

 48 Axial velocity along jet center line at two different instants, using either Weakly Compressible SPH method either an incompressible Finite Volume method.

33 Figure 4 . 9 :

 3349 Transverse profiles of axial velocity, at x = 9D and two different instants, using either Weakly Compressible SPH method either an incompressible Finite Volume method.

Figure 4 .

 4 Figure 4.10: State-of-the-art chronology of SPH-FV coupling

Figure 4 . 11 :

 411 Figure 4.11: SPH domain in Kumar's SPH-FV coupling method. Interfacial water and air SPH particles are shown in black with the supporting neighbor SPH particles shown in gray. Grey neighbor particles are used to avoid kernel function truncation over the interfacial SPH particles during the SPH simulation. Figure is taken from [159].

Figure 4 . 13 :

 413 Figure 4.13: Configuration of Global Domain (GD) and Zonal Domain (ZD) for a plane jet in a coflow following Aristodemo et al. configuration [4].

n

  x and n y stand for the number of cells in x-and y-directions respectively.

Figure 4 .

 4 Figure 4.14 shows the passive scalar γ field at tU/D = 6 for the three previous resolutions.It can be observed that head of the jet is diffused (brown color) even with the finer mesh. Only fine mesh field shows a distinctive jet head, with a "mushroom-head" shape. To reduce the diffusion of γ, it is therefore necessary either to refine again the mesh, thus increasing the computational cost, either to correct the field with a Lagrangian formalism, hence the SPH-FV coupling. The next SPH-FV simulation will be performed using the fine refinement in FV mesh.

Figure 4 . 14 :

 414 Figure 4.14: Passive scalar γ field at tU/D = 6 for three different resolutions in Finite Volume. Coarse, medium and fine meshes own respectively 40 × 20, 80 × 40 and 160 × 80 cells.

Figure 4 .

 4 Figure 4.15 shows evolution of the passive scalar field without (left) and with (right) a zonal SPH correction. As stated previously, without the SPH correction, the scalar field is diffused, as it can be observed from tU/D = 2 to tU/D = 10. The Zonal SPH γ field shows, as expected, only two values: γ = 0 for the steady current and coflow, and γ = 1 for the jet coming outside the nozzle. No diffusion is observed in the upper part of figures (2) because of the Lagrangian nature of SPH. At tU/D = 6, the SPH jet leaves the domain without notable impact of FV-SPH interface on the flow.

Figure 5 . 1 :

 51 Figure 5.1: Schematic of the injector used by Stepowski et al. [5].

Figure 5 . 2 :

 52 Figure 5.2: Dimensions and boundary conditions of the computational domain.The zonal domain, with medium refinement, is shown in yellow. The global domain, with coarse refinement, is shown in black. Γ stands for the zonal interface with the global domain.

Figure 5 . 3 :

 53 Figure 5.3: Liquid inlet patch faces for three different mesh refinement.

4 . 4

 44 for more details. Variables that are interpolated from zonal field to underlying global field in the restriction step (see part 3.4.5) are velocity U , volume fraction α and volumetric face fluxes F . Divergence free and mass conservation correction steps are performed after the restriction step, as well as interface geometric characteristics updating (see part 3.4.6).

Figure 5 . 4 :

 54 Figure 5.4: Evolution of computed mean gas flux divided by mean gas flow rate, in both domains of the zonal simulation.

Figure 5 . 5 :

 55 Figure 5.5: (a) CPU Time by physical time VS number of cores. Thick lines represent ideal scaling. (b) Efficiency for each simulation taking as reference the one with the least number of cores.

  (a) Mean liquid volume fraction and (b) liquid volume fraction variance. Values are averaged in space considering the whole main domain. Instantaneous liquid structures of medium RI and medium TDF simulations are shown in figure 5.7 with the isosurfaces α = 0.5. In 5.7-(a), showing structures obtained with RI model, the influence of pressure in liquid detachments is highlighted. Over pressure destabilizes and provokes separation of structures from the liquid core. This behavior seems absent when looking at the TDF model snapshot in 5.7-(b). Similarly, RI structures obtained with the medium zonal RI and fine zonal RI l simulations are shown respectively in figures 5.8-(a.1) and 5.8-(b.1). Medium zonal RI simulation shows similar structures to those obtained with the medium RI simulation. The dynamic pressure field is as well similar. Structures are cut by the zonal domain right interface Γ which defines the end of the region governed by RI model. Underlying structures in global domain are shown in figures 5.8-(a.2) and 5.8-(b.

Figure 5 . 7 :

 57 Figure 5.7: Three-dimensional snapshots of phase indicator isosurface α = 0.5, along with the dynamic pressure field.

( a )

 a Obtained with a medium mesh and RI model; (b) obtained with a medium mesh and TDF model.

5. 6 . 3 . 1 Figure 5 .

 6315 Figure 5.11 shows the mean volume fraction fields, from the two medium TDF and medium RI simulations, the two zonal simulations (medium zonal RI and fine zonal RI ) and the experiment measurements.

196CHAPTER 5 .Figure 5 . 10 :Figure 5 . 11 :

 5510511 Figure 5.10: Instant liquid volume fraction fields. Isocontour α = 0.5 is shown with black lines when RI model is used. Interface of the zonal domain is shown with white rectangle. RI and TDF stand for resolved interface and turbulent diffusive flux models respectively.

5. 6 201 Figure 5 . 15 :

 6201515 Figure 5.15: Mean interface density Σ field in global coarse domain obtained with fine zonal run.

Figure 5 . 16 :

 516 Figure 5.16: Evolution of volume of liquid using the zonal grid solver.

Figure 5 . 17 :

 517 Figure 5.17: Instantaneous velocity field in global coarse domain obtained with fine zonal run.Fluxes going in and out of zonal domain are shown in black arrows.

Figure 5 .

 5 Figure 5.17 shows an instantaneous velocity field in coarse GD obtained whit the fine zonal RI simulation. It can be observed numerical staggered oscillations above and below zonal domain. These oscillations are normal to the zonal boundaries. Along upper and lower interfaces, fluxes are going inside ZD, as shown with black arrows in figure5.17. These velocity oscillations may be thus explained by the non conservation of momentum in the normal interpolation scheme of velocity in prolongation step (see section 3.4.4). The normal interpolation scheme brings

Figure 5 . 18 :

 518 Figure 5.18: LES instantaneous turbulence morphology in zonal and global domains obtained with fine zonal run.

Field

  of second invariant of ∇U is shown with color map. Isosurfaces at 10 8 s -2 cut by z axis plane are shown in black.

Figure 5 .

 5 Figure 5.18 shows iso-contours of the second invariant of the velocity gradient, namely Qcriterion, in Zonal Domain. It can be seen how the upper and lower GD-ZD interfaces (Dirichlet condition) interact with the fluid flow by retarding the motion tangentially to the surface. This phenomenon is typical close to a wall because of the viscous shear [173]. On the other hand, just upstream right interface, structures are advected by the flow without notable influence of the boundary thanks to the Neumann condition.

Figure 5 . 19 :

 519 Figure 5.19: Dimensions and boundary conditions of the extended computational domain.

5. 8 7 Figure 5 . 20 :

 87520 Figure 5.20: Liquid volume fraction fields at three different instants.

  (a), (c) and (e): obtained with very coarse TDF extended configuration; (b), (d) and (f): obtained with medium zonal RI extended configuration.

Figure A. 1 :

 1 Figure A.1: Test method to known if the point P is inside the cell i.

•

  A first loop is performed over all ZD internal faces. Each internal face f Z owns a owner cell P Z and neighbor cell N Z (see configurations (a), (b), (e) and (f) in figure A.2).Owner cell P Z is associated to an acceptor GD cell, noted P G and neighbor cell N Z is also associated to an acceptor GD cell, noted N G . These informations are available since cell center restriction algorithm has already been performed. Face f Z is an eligible donor face if P G and N G are different. In other word, if face f Z is not located inside a GD cell but at the edge between two GD cells (configurations (a) and (e) in figure A.2). Configurations (b) and (f) in figure A.2 show a zonal face located inside a global cell.

Figure A. 2 :

 2 Figure A.2: Height possible position configurations for a face f Z located in Zonal Domain (ZD) and a face f G located in Global Domain (GD).

A. 3 Face center restriction 223 N

 3223 Subscripts () Z and () G respectively stands for ZD and GD. An internal face shares an owner cell P and a neighbor cell N . A patch face (on the domain boundary) is only owned by P . Configurations where an association between a zonal face and global face is possible are configurations (a), (c), (e) and (g) because faces are coincident.acceptor cell P G . Virtual neighbor cell center N virt,Z is computed by using distance between patch face center C f,Z and owner cell centroid P Z , with following relation: virt,Z = C f,Z + β (C f,Z -P Z ) , (A.3)

3 Figure A. 3 :

 33 Figure A.3: Sending map and received map examples with 4 processors.

  Possibility of arrangements for two independent grids in DDM techniques. . . . .3.4Configuration of a zonal embedded grid in a turbulent channel flow. . . . . . . .3.5The face f whose owner is cell center P and neighbour cell center N . . . . . . . .3.6Algorithm structure of both single grid two-phase solvers. . ... . . . . . . . . . 3.7 Global and zonal domains. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.8 Zonal methodology algorithm. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.9 Interface Γ between Zonal Domain (ZD) and Global Domain (GD) for a mesh resolution ratio r x of 2:1. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.10 Three types of interpolation between Zonal Domain and Global Domain. . . . . . 3.11 Simulation domain, boundary conditions and initial configuration of Hysing et al. [2] rising bubble problem. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . Zoom on the fine zonal mesh near interface. . . . . . . . . . . . . . . . . . . . . . 100 3.16 Transient state liquid volume fraction fields obtained with two zonal runs. . . . . 102 3.17 TDF model: Steady state volume fraction and velocity fields obtained with zonal run. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 102 3.18 TDF model: Relative difference between two steady state velocity fields in coarse mesh. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 103 3.19 TDF model: Velocity and liquid volume fraction profiles along jet center line. . . 104 3.20 TDF model: Evolution of volume of liquid using the zonal grid solver. . . . . . . 105 3.21 RI model: Steady state volume fraction and velocity fields obtained with zonal run. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 105 3.22 RI model: Relative difference between two steady state velocity fields in coarse mesh. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 106 3.23 RI model: Velocity and volume fraction profiles along jet center line. . . . . . . . 107 3.24 Hybrid model: Steady state volume fraction and velocity fields obtained with zonal run. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 108 3.25 Hybrid model: Steady state velocity and liquid volume fraction profiles along jet center line. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 108 3.26 Evolution of bubble rising velocity for two different face interpolation schemes of phase indicator. . Velocity profile along jet center line, using either Dirichlet either inletoutlet coupled boundary condition for velocity in zonal grid. . . . . . . . . . . . . 119 3.36 Evolution of bubble rising velocity with three different types of coupled boundary conditions for velocity in zonal grid. . . . . . . . . . . . . . . . . . . . . . . . . . 120 3.37 RI model: Velocity profile along jet center line for three different zonal domain sizes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 121 3.38 RI model: Velocity relative difference in each cell between two domains, with coarse refinement. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 122 3.39 Temporal evolution of relative mass error in rising bubble test case, with and without phase indicator correction along interface Γ. . . . . . . . . . . . . . . . . 3.42 Relative difference of cell center face flux before and after face flux correction step.127 3.43 RI model: Velocity relative difference in each cell between two domains, with coarse refinement, with and without divergence free correction procedure. . . . . 3.44 RI model: Velocity profile along jet center line, with and without divergence free correction procedure. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.45 Possibilities of processor arrangements in Global Domain and Zonal Domain, here with 4 processors. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.46 Example of strong speed-up profile for a parallelized solver. . . . . . . . . . . . . 3.47 Parts of the zonal methodology algorithm that have been parallelized. . . . . . . 3.48 Liquid-gas interface at t = 3 s of Hysing skirted bubble configuration [2] obtained with zonal simulations using a different number of processors. . . . . . . . . . . . 3.49 Evolution of bubble rising velocity obtained with zonal simulations using a different number of processors. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

	d e f h M m p Q t 3.1 3.15 3.33 3.34 3.35 RI model: LIST OF FIGURES number of dimensions total energy cell face smoothing length Mach number mass kinematic pressure source term time Temporal evolution of cumulated clipped mass in the liquid-air jet configuration. 117 --M 2 .T -2 m 2 s -2 --L m -1 M kg M 2 .T -2 m 2 s -2 --T s LIST OF FIGURES 117 Mass error evolution in bubble rising configuration using either coupled gradient either zero gradient for coupled inlet-outlet boundary condition in zonal grid. . . 118 3.41

Three types of AMR methods. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.2 Block-based time-subcycled AMR algorithm of Martin et al. [1], for two levels of refinement. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.3 3.12 Liquid-gas interface at t = 1.5 s and t = 3 s for three simulations of Hysing skirted bubble configuration [2]. . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.13 Evolution of bubble rising velocity. . . . . . . . . . . . . . . . . . . . . . . . . . . 3.14 Configuration of the liquid-air jet configuration. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 110 3.27 Temporal evolution of relative mass error in rising bubble test case for two different face interpolation schemes of phase indicator. . . . . . . . . . . . . . . . . 111 3.28 Evolution of bubble rising velocity for different interpolation schemes in time with refinement r x = 2. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 112 3.29 Evolution of bubble rising velocity for different tangential interpolation schemes with refinement r x = 2. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 115 3.30 RI model: Velocity profile along jet center line for different tangential interpolation schemes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 115 3.31 TDF model: Velocity profile along jet center line for different tangential interpolation schemes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 116 3.32 Evolution of bubble rising velocity using either coupled gradient either zero gradient for coupled inlet-outlet boundary condition in zonal grid. . . . . . . . . . . Simulation domain of Hysing et al. [2] rising bubble problem with different size and placements of zonal domain. . . . . . . . . . . . . . . . . . . . . . . . . . . . 122 3.40 Evolution of bubble rising velocity for different emplacements and sizes of the zonal grid. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 123 4.1 Eulerian and Lagrangian representation of fluid flow equation. Figure from [3]. . 4.2 Illustration of wall modeling by using ghost particles. . . . . . . . . . . . . . . . 4.3 Comparison of velocity profiles for a low Reynolds Poiseuille flow obtained with a Weakly Compressible SPH simulation and an analytical solution. . . . . . . . . 4.4 SPH velocity field obtained on the low Reynolds Poiseuille flow configuration. . . 4.5 Laminar jet in a coflowing environment . . . . . . . . . . . . . . . . . . . . . . . 4.6 Evolution of the phase field in a laminar jet in a coflow configuration, obtained with Weakly Compressible SPH. . . . . . . . . . . . . . . . . . . . . . . . . . . . 4.7 Evolution of the phase field in a laminar jet in a coflow configuration, obtained with an incompressible finite volume solver. . . . . . . . . . . . . . . . . . . . . 4.8

  Description of a coupled inlet-outlet boundary condition at interface Γ in ZD for a variable φ. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3.2 Physical properties of the rising bubble test case. . . . . . . . . . . . . . . . . . . 3.3 Two-phase numerical simulations performed in the rising bubble configuration. . 3.4 Properties of liquid and air in liquid-air jet configuration. . . . . . . . . . . . . . 3.5 Types of RANS performed in the liquid-air jet configuration. . . . . . . . . . . .

	2.1	Complexity of different solvers for the two-dimensional Poisson problem. . . . . .
	3.1

4.1 Three different mesh refinements for the plane jet in a coflow configuration in Finite Volume. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5.1 Simulated flow conditions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5.2

.59) 2.8 Solution of linear equation systems 47 It

  is to note that only non-orthogonal correction term stays explicit in equation 2.58 as shown in section 2.6.2. It is thus considered as a source term. This implicit method guarantees the boundedness of the solution and is unconditionally stable, even if the Courant number limit is violated.

	• Crank-Nicholson method (Eq. 2.44), second order accurate, expresses RHS of equation
	2.53 as a function of both former values (at t n ) and new values (at t n+1 ):

CHAPTER 2. FINITE VOLUME METHOD 2.8.0.1 Implicit system

		.62)
	where a P is a CV coefficient, a N neighbor CV coefficients and B P , CV source term. Neighbor
	term and source term can be combined together in RHS of equation 2.62 into a single source
	term. Now, considering all CVs of the discretized computational domain, one obtains a system
	of algebraic equations in the following form:
	[φ] = [B] ,	(2.63)
	where [φ] is the vector of φ-s for all CVs and [B] is the source term. Solving this system is
	explicit and direct and does not iterations. But it is unstable if the Courant Number Co is
	greater than one. Thus, implicit methods are preferred. it involves solving implicitly an alge-
	braic equation system.

.92) 2.11 Discretization of the Navier-Stokes equations 55 where H(U )

  is a function of last known solution for velocity, i.e.

	-For first PISO loop,
	predicted velocity U m = U * if step (1) has been performed,
	velocity at previous time-step U m = U n otherwise,
	-Otherwise, solution U m = U m from step (6).
	Corresponding code is:
	volScalarField rAU(1.0/UEqn.A());
	volVectorField HbyA("HbyA", U);
	HbyA = rAU*UEqn.H();
	(3)

Computing pseudo-volumetric face flux:

	A pseudo-volumetric face flux is computed based on pseudo-velocity Ũ interpolated to
	face f .
	F = Ũ f • S .	(2.93)
	Corresponding code is:
	surfaceScalarField phiHbyA
	(
	"phiHbyA",
	(fvc::interpolate(HbyA) & mesh.Sf())
	+ fvc::interpolate(rAU)*fvc::ddtCorr(U, phi)
	);
	(4)

Adjustment of outflow on boundary conditions:

	When no Dirichlet boundary conditions are imposed to pressure field, outlet fluxes are
	adjusted to obey continuity, which is necessary for creating a well-posed problem where
	a solution exists for pressure. Outlet fluxes are adjusted so that everything that goes in
	the computation domain is equal to what goes out:

2.12 Multigrid methodology

  t n → t n+1 .

	First developed in the late 1970s by Achi Brandt [66] to address the solution of elliptic equa-
	tions, multigrid is classified among iterative methods as Gauss-Seidel iterations, Successive
	OverRelaxation (SOR), Conjugate gradient or Fast Fourier Transform (FFT) (see section 2.8).
	Multigrid is the most efficient solver regarding computational cost, as it is shown in a classifi-
	cation from [67] (see table 2.1) of the different methods by their associated computational costs
	to solve a linear two-dimensional Poisson equation. Multigrid acceleration of the Gauss-Seidel
	point-iterative method is currently the solution algorithm of choice for commercial CFD codes.
	Method	# operations
	Gaussian elimination	O(N 2 )
	Jacobi iteration	O(N 2 log )
	Gauss-Seidel iteration	O(N 2 log )
	Successive overrelaxation (SOR) O(N 3/2 log )
	Fast Fourier Transform (CG)	O(N log N )
	Multigrid (iterative)	O(N log )
	Full Multigrid (FMG)	O(N )
	nCorrectors PISO loops
	Figure 2.7: PISO algorithm in icoFoam solver for one time-step

Table 2 .

 2 1: Complexity of different solvers for the two-dimensional Poisson problem.

  PISO loop index () m is introduced in the following. m is the last known solution for velocity, i.e. * For first PISO loop, U m = U * if step (2) (momentum predictor) has been performed, U m = U n otherwise, * Otherwise, solution U m from step (5.5).

	(5.1) Computing pseudo-velocity:
	So-called pseudo-velocity is computed without pressure and source terms contribu-
	tion:	Ũ =	H(U m ) a P	,	(3.39)
	where U

) . (3.38) FLOWS (5) PISO loop is solved N corr times to obtain solutions for U n+1 and P n+1 rgh :

  Before interpolating from one domain to another, it is necessary to interpolate cell centered fields to face centers. Variables that are already face centers, i.e. a surface normal gradient ∇ ⊥ φ, do not necessitate this step. A surface normal gradient is the component, normal to the face, of the gradient of values at the centers of the two cells that the face connects.

			(2.2) Single grid solver
			for one ZD time step
			(see figure 3
		(2.1) Update of ZD	r
	(1) Single grid solver	boundary conditions by
	for one GD time step	interpolation of GD fields
	(see figure 3.6)
			(U, P rgh , α, φ) n+ 2 r
			(U, P rgh , α, φ) n+1

• (step 2.1.2) interpolation in time,

• (step 2.1.3) interpolation tangential to the zonal interface.

The first step (2.1.1) depends on the variable that is interpolated. The two others are generic. Let us detail these procedures below. step (2.1.1) In GD, cell centered fields are interpolated to face center f :

Velocity:

Cell centered velocity field is interpolated with a linear scheme and a correction is added to ensure mass conservation. It consists to add to velocity vector magnitude the difference Global Domain (GD) Zonal Domain (ZD) (U, P rgh , α, φ) n (U, P rgh , α, φ) n (U, P rgh , α, φ) n+1 (U, P rgh , α, φ) n+1,corr (U, P rgh , α, φ) n+ 1

Table 3 .

 3

1: Description of a coupled inlet-outlet boundary condition at interface Γ in ZD for a variable φ.

Table 3 .

 3 2: Physical properties of the rising bubble test case.

	1000	1	10	0.1	0.98	1.96	35
			no-slip wall
			Ω 1
					slip wall

Table 3 . 4

 34

: Properties of liquid and air in liquid-air jet configuration.

Table 3 .

 3 5: Types of RANS performed in the liquid-air jet configuration.

	Configurations		Main (global) domain		Zonal domain
		Mesh ref. Mesh size Two-phase model Mesh ref. Mesh size Two-phase model
	Coarse TDF	Coarse	3k cells	TDF model	-	-	-
	Fine TDF	Fine	10k cells	TDF model	-	-	-
	Zonal TDF	Coarse	3k cells	TDF model	Fine	4k cells	TDF model
	Coarse RI	Coarse	3k cells	RI model	-	-	-
	Fine RI	Fine	10k cells	RI model	-	-	-
	Zonal RI	Coarse	3k cells	RI model	Fine	4k cells	RI model
	Zonal Hybrid	Coarse	3k cells	TDF model	Fine	4k cells	RI model

  is velocity field, p is the kinematic pressure field and γ passive scalar field. Subscript () n is index for time instant t and () n + 1 stands for time instant t + ∆t after one time step.

	Global Domain (GD)	Zonal Domain (ZD)
	(U , p, γ) n	(U , p, γ) n
	(2) Update of ZD bound-
	ary conditions by inter-
	polation of U from GD
	(1) FV single grid	(3) SPH single grid
	solver	solver
	(U , p, γ) n+1	(U , p, γ) n+1
	(4) Transfer of ZD
	fields (U and γ) to
	GD by interpolation
	Prolongation on GD/ZD boundaries P
	Restriction R
	Figure 4.12: Finite volume-SPH zonal coupling algorithm.
		.84)

U

  Configuration of Aristodemo et al.[START_REF] Aristodemo | Sph modeling of plane jets into water bodies through an inflow/outflow algorithm[END_REF] is chosen for testing the hybrid SPH/Finite Volume solver, since SPH simulation alone has shown good ability to solve advection of a passive scalar (inlet phase) in previous validation (see part 4.3.2 and figure 4.6). Indeed, one of the major strength of SPH is its convective nature: convective transfer of physical parameters such as mass, momentum, velocity, energy, etc., is simulated natively by the motion of the nodes/particles. The non linear convective term is thus excluded from the Lagrangian governing equations, as shown below in the transport equation of a passive scalar γ:

		Dγ Dt	= 0 .	(4.88)
	While, in Eulerian formalism, convection term appears:
	∂γ ∂t	+ ∇ • (γU ) = 0 .	(4.89)
	Semi-discretized in finite volume formalism, equation (4.89) becomes

table 4

 4

	.1.
	FV Refinement n x × n y Number of cells
	Coarse	40 × 20	800
	Medium	80 × 40	3200
	Fine	160 × 80	12800

Table 4 .

 4 1: Three different mesh refinements for the plane jet in a coflow configuration in Finite Volume.

  .[START_REF] Aristodemo | Sph modeling of plane jets into water bodies through an inflow/outflow algorithm[END_REF] plays an important role in destabilization of the liquid jet and in the liquid core length. Values of the previous characteristic non-dimensional numbers are reported in table 5.1.

	U g (m/s) U l (m/s) W e Re g	Re l	J
	115	1.3	500 8000 2600 10
	Table 5.1: Simulated flow conditions.

Table

  The above mentioned estimations gives the minimum mesh size near the gas nozzle ∆ x | 0D l = 39µm. Medium and fine mesh refinements are thus sufficient to capture vortexes near the gas nozzle with LES. Coarse mesh refinement is not sufficient in this region Refinement Cells at liquid nozzle exit Cell size near gas and liquid injectors exit

	Coarse	12	75 µm
	Medium	24	38 µm
	Fine	48	19 µm

  have been performed. Their meshes sizes and two-phase model employed are sum up in table 5.3.

	Configurations		Main (global) domain			Zonal domain
		Mesh ref. Mesh size Two-phase model Mesh ref. Mesh size Two-phase model
	Coarse RI	Coarse	260k cells RI model	-	-	-
	Coarse TDF	Coarse	260k cells TDF model	-	-	-
	Medium RI	Medium	2.1M cells RI model	-	-	-
	Medium TDF	Medium	2.1M cells TDF model	-	-	-
	Medium zonal RI Coarse	260k cells TDF model	Medium	690k cells RI model
	Fine zonal RI	Coarse	260k cells TDF model	Fine	5.5M cells RI model

Table 5 .

 5

3: LES performed in the coaxial atomizer configuration of Stepowski et al.

[START_REF] Stepowski | Measurement of the liquid volume fraction and its statistical distribution in the near development field of a spray[END_REF]

.

  To eliminate the initial transient part, time averaging process is started after 3 liquid advection time tU l /D l , that corresponds to 150 gas advection times tU g /D g . Convergence of each simulation is monitored with evolution of field average mean and variance volume fraction values, which are respectively reported in figures 5.6-(a) and 5.6-(b). Correct convergence is obtained after 72 tU l /D l , for both mean and variance values. Fluctuations and variations are though still observable. To obtain complete convergence, simulations should have been run on a longer period, which has a non negligible computational cost. It is indeed hardly achievable in numerical to obtain more than 1000 independent samples as it can be done in experimental. For the sake of computational saving, medium TDF simulation has been run on a shorten time lapse since it is clear before convergence that results are far from experience results. Fine zonal RI simulation, which is the most costly case, has been run as well on a shorten period, until 54 tU l /D l . PRIMARY ATOMIZATION

										0.0016
		0.10								0.0014
	Mean volume fraction	0.06 0.07 0.08 0.09					coarse TDF coarse RI medium TDF medium RI medium zonal RI fine zonal RI	Volume fraction variance	0.0002 0.0004 0.0006 0.0008 0.0010 0.0012					coarse TDF coarse RI medium TDF medium RI medium zonal RI fine zonal RI
		10	20	30	40 tUl/Dl	50	60	70		10	20	30	40 tUl/Dl	50	60	70
					(a)							(b)
					Figure 5.6: Monitoring of time convergence.

5.6 Results 193 5.6.3.2 Quantitative results

  Figures 5.12 and 5.13 respectively show the axial and radial profiles obtained with three simulations using RI model in the primary atomization zone. The medium zonal RI profiles are here in good agreement with the medium RI ones, as previously stated with qualitative results, meaning that the coupling does not affect the flow in the zonal domain. A slight difference can be observed on radial profile peak at x/D = 1.91. It is due to a lack of convergence of the medium RI simulation further from the injector, as previously observed with mean α field (figure5.11-(b)). The medium RI and medium zonal RI simulations estimate relatively well the experimental liquid core penetration, as shown in axial profiles, figure 5.12. At x = 1D l , radial profiles are also in good agreement with experimental results, but it is not the case further at x = 1.47D l and x = 1.91D l , where numerical results overestimate the mean liquid volume fraction.

  5.10-(b)). Now, with the zonal approach, we chose to place a boundary at x = 3D l from which the flow is solved not any more with RI model but with TDF model. This choice is arbitrary and based on experimental axial profile. In medium zonal RI and fine zonal RI fields (figures 5.10-(c) and 5.10-(d) respectively), one can observe unresolved droplets just before this boundary, meaning that mesh is not fine enough in this region. One can also observe the biggest structures crossing the RI-TDF interface. After the interface, the structure is physically diffused by diffusion at a relatively high rate. Thus, one could discuss the assumptions made in TDF model and the parameters attached to the turbulent diffusion, as turbulent Schmidt number value (0.7 in this configuration). This discontinuity is not observed with mean α fields, as shown in figures 5.11-(c) and 5.11-(d). Low volume fractions isocontours, in orange, are physically correct.

Table 5 .

 5 .4 below. 4: Measured CPU gain between medium zonal RI and medium RI simulations.It is slightly lower with 58% (speedup of 2.4). The coupled approach must probably lower the global time-step because of the CFL constraint, that is more important when the liquid has reached the GD-ZD interface. It hence increases weakly the computational cost. Nevertheless, this speedup of 2.4 is

	Configuration	Number CPU effort per	Measured gain Parallel Gain reported
		of cores physical 10 -ms (32 processors) efficiency to 1 processor
	Medium RI	32	1, 230 h		0.75
	Medium zonal RI	32	520 h	58%	0.65	63%

a good result which shows one of the main interest of this zonal approach, i.e. to lower the computational cost of atomization process numerical simulation.

  Concerning the fine zonal RI simulation, it can not be compared to a fine RI simulation since it has not been performed. We can however estimate this gain, as shown in next paragraph.

Table 5 . 5

 55

	5.6 Results

: Estimated CPU gain between medium zonal and medium simulations in (a) and fine zonal and fine simulations in (b).

Table 5 .

 5 .6. 6: LES configurations using a combustion chamber size domain in the coaxial atomizer configuration of Stepowski et al.[START_REF] Stepowski | Measurement of the liquid volume fraction and its statistical distribution in the near development field of a spray[END_REF].

	Configurations		Main (global) domain			Zonal domain
		Mesh ref.	Mesh size	Two-phase model Mesh ref. Mesh size Two-phase model
	Medium TDF extended	Medium	15.5M cells TDF model	-	-	-
	Very coarse TDF extended Very coarse 1.1M cells	TDF model	-	-	-
	Medium zonal RI extended Very coarse 1.1M cells	TDF model	Medium	1.1M cells RI model

Table 5 .

 5 7: Measured CPU gain between large zonal and standard runs using a medium effective mesh resolution near the injector.The measured gain is reported in table 5.7. The gain is of 97%, i.e.

	Configuration	Number CPU effort for Measured gain
		of cores physical 1.2 µs (12 processors)
	Medium TDF extended	12	1, 372 s	-
	Medium zonal RI extended	12	42 s	97%

a speedup of 33 be- tween the medium zonal RI extended and the medium TDF extended simulations.

SPH solution is advanced for one time-step, only for interfacial particles (black particles in figure4.11), keeping grey particles as fixed boundary conditions. These grey particles can be considered as dummy particles (see section 4.2.4.6).

3 Non-interfacial SPH particles (grey particles in

figure 4.11) are updated based on current global domain FV state.

RI and TDF stand for resolved interface and turbulent diffusive flux models respectively.

Remerciements

Le travail présenté dans ce manuscrit est le fruit de la collaboration entre le CORIA (COmplexe de Recherche Interprofessionnel en Aérothermochimie) et le LOMC (Laboratoire Ondes et Milieux Complexes). Il a été financé par le CNRS (Centre National de la Recherche Scientifique) à travers le projet EMC3 (Energy Materials and Clean Combustion Center) du Programme d'Investissements d'Avenir du gouvernement français. Je tiens à remercier chacun de ces organismes de m'avoir permis de réaliser c'est grâce à vous deux. Je remercie Nicolas Hecht du LOMC avec qui j'ai collaboré contribution au couplage SPH/Volumes Finis. Ca a été un plaisir de travailler ensemble. Merci également à Grégory Pinon du LOMC et Mostafa Safdari Shadloo de l'INSA de Rouen pour vos conseils et votre aide sur la partie SPH. Merci à Vuko Vukcevic pour m'avoir permis de paralléliser le solveur couplé dans le cadre de NUMAP-FOAM School 2017. Je souhaite remercier Cédric Chamberlan, Guillaume Edouard et Alexandre Poux pour votre aide et votre expertise qui m'ont permis d'avancer (parfois plus vite, parfois d'être débloqué)

Water interface and walls are respectively shown in blue and black lines. The finer Zonal Domain (ZD) is not coupled until t 2 when the wave reaches the sloping beach.

Appendix A Donors/acceptor associations in the zonal algorithm

Algorithm dedicated to the association of donors and acceptors for face center prolongation, cell center restriction and face center restriction are described in this part. These three algorithms are called once at the beginning of the simulation and do not need to be called again since meshes are not moving.

When association of donors and acceptors is done, all pairs are stored in a list local to each acceptors processor. This list will be used during simulation for distributing scalar and vector fields between processors and perform prolongation and restriction interpolations.

In each of these algorithms, processes for distributing data between processors are performed several times. This type of procedure is detailed in the last subsection.

A.1 Face-patch prolongation

The acceptor faces are located in Zonal Domain, more precisely at interface Γ. Interface constitutes boundary conditions coupled with GD internal field, for Zonal Domain. A face located in a boundary condition is called patch face. Thus, number of acceptor patch faces is already known, in each ZD sub-domain (processor), as well as number of donor internal faces in each GD sub-domain. Donors may also be patch faces if one processor patch part is coincident with ZD interface.

To ease the parallelization work, only the first order tangential interpolation scheme named injection is considered in the parallelized version. Thus, one acceptor patch face is associated with one donor internal face (or processor patch face).

The different step of the algorithms are detailed below.

• 1 st step (stage 1 in algorithm) consists to store acceptor informations: index, processor number, location coordinates and patch index.

• 2 nd step (stage 2 in algorithm) consists, for each processor, to known the number of acceptors to send to other processors. The criteria is: Is this acceptor face center inside ALGORITHM

• ω d = 1 if donor face normal n f and acceptor face normal n f,G are collinear and donor face is an internal face.

• ω d = -1 if donor face normal n f and acceptor face normal n f,G are not collinear and donor face is an internal face. It means that donor flux value will be inversed to take in account this non-collinearity.

• ω d = 0.5 if donor face normal n f and acceptor face normal n f,G are collinear and donor face is a processor face. It means that donor value will contribute twice to the acceptor value, since a same quantity is located on two processor patch faces. If it is a flux, it is also inversed from one patch face to the other, since normals are in inverse directions. To remedy this, value shall be divided by two.

• ω d = -0.5 if donor face normal n f and acceptor face normal n f,G are not collinear and donor face is a processor face.

Third step to deal with is the case of a patch face acceptor. Neighbor acceptor cell does not exists, thus acceptor face f is searched by means of the least distance between face candidates and considered donor face. Face candidates are all patch faces in GD (processor patch and boundary condition patch. Once the closest patch face is found, its corresponding patch index is derived. Finally, similarly to the last part of second step, weight coefficient ω d is computed depending on collinearity between donor and acceptor face normals. Thus, its value is either 1, either -1. A donor processor face will not have influence on weight coefficient here because there are also two acceptor processor faces. Thus, contribution of a donor processor face will be unique for each acceptor processor face.

A.4 Distributing data between processors

Distributing data between processors is a recurring process in the previous association algorithms and the interpolation algorithms. It is performed with parallel communication function distribute, from OpenFOAM R library mapDistribute class, that uses MPI protocole.

Computing a distribute map requires to assemble two maps for each processor: a sending map and a received map. A map is a list of lists with different sizes. There is any many lists than there is processor domains. Each list contains element (cell, face, etc...) indexes. A sending map will thus store all element indexes being sent by this processor to other processors. A received map is simply an index offset by the number of values received by previous processors. An example of these two maps is given in figure A.3.

To known the number of values that a processor receives from all other processors, the MPI gather and scatter functions are used. Gather function consists to takes elements from all processors and gathers them to one single processor, that is often master processor. Thus, all informations that were previously dispatched among all the processors are know regroup on one single processor.

STAGE 3 : Count number of acceptors received

Count number of points I'm receiving from all other processors. Gather/scatter number of acceptor points going to each processor from each processor so that all processors have all necessary information when creating the map distribute tool for distributing acceptor points. Gather and scatter functions are from Pstream class and call MPI C++ functions.

STAGE 7 : Create sending map for donors

Now that donors/acceptor pairs have been set up, next stages from stage 7 to stage 10 are the inverse way of stages 2 to stage 5. Sending map for donors is basically the constructing map for acceptors since we have used the same addressing for donor search. Create a copy from map distribute object used to communicate acceptor data. The size of map does not change since we consider package of donors to send for each acceptor. labelListList sendDonorMap = acceptorDistribution.constructMap();

STAGE 8 : Count number of donors received

Reuse nAcceptorsToProcessorMap[i][j], which tells me how many acceptors processor i is sending to processor j. The number of donors received by processor j is the same as the number of acceptors sent to processor j.

STAGE 11: Filter possibly multiple remote donors

If for a given acceptor, donors are located on different processors, a donors/acceptor pair will be received several times on this processor. Goal of this stage is to combine these pairs and avoid duplicates. New list without duplicates is named combinedDonorAcceptorList.

B.2 Distribution of donor field values

This function is necessary for interpolation. It creats list containing number of donors this processor is sending to other processors. • Create a a Hash table used to send unique donors since a single donor can be used for multiple acceptors. Note : it is not the case in restriction interpolation step, a single donor is used by a single acceptor, but it is kept from overset structure and done in a general way.

List<labelHashSet> sendMap(Pstream::nProcs());

• Create labelList containg donor indices which will be used to create remote donor to local acceptor addressing.

labelList donorIDs(donorMesh.nCells(), -1);

• Create sending map and initialize the capacity as nDonorsByAcceptor times the number of donors for this processor with nDonorsByAcceptor being equal to how many donors an acceptor can have at maximum. For regular mesh ratio, this number will mesh ratio square in two dimension and mesh ratio cube in three dimensions.

STAGE 4 : Create remoteDonorToLocalAcceptor addressing object

Now that we have a distribute map, given any donor field, we will receive donor values from other processors, but donor index from donors/acceptor pair is not the same than in received donor field. Thus, it is necessary to create a addressing object to convert local donor index to a distributed index.

• First initialize the remote object which is a list (for n processors) of label fields (donor indices).

remoteRestricDonorToLocalAcceptorAddrPtr_ = new List<labelField>(Pstream::nProcs()); List<labelField>& rdlaAddr = *remoteRestricDonorToLocalAcceptorAddrPtr_;

• Each processor needs to know how many cells we have in all other processors. labelList procNCells(Pstream::nProcs()); procNCells[Pstream::myProcNo()] = donorMesh.nCells(); Pstream::gatherList(procNCells); Pstream::scatterList(procNCells);