# CFD Model

## 1. Notations and units

Notation Quantity Unit

$\rho_f$

fluid density

$kg \cdot m^{-3}$

$\boldsymbol{u}_f$

fluid velocity

$m \cdot s^{-1}$

$\boldsymbol{\sigma}_f$

fluid stress tensor

$N \cdot m^{-2}$

$\boldsymbol{f}^t_f$

source term

$kg \cdot m^{-3} \cdot s^{-1}$

$p_f$

pressure fields

$kg \cdot m^{-1} \cdot s^{-2}$

$\mu_f$

dynamic viscosity

$kg \cdot m^{-1} \cdot s^{-1}$

$\bar{U}$

characteristic inflow velocity

$m \cdot s^{-1}$

$\nu$

kinematic viscosity

$m^2 \cdot s^{-1}$

$L$

characteristic length

$m$

## 2. Equations

Navier-Stokes model is used to model incompressible Newtonian fluid. It can be described by these conservative laws :

Momentum conservation equation
$\rho_{f} \left. \frac{\partial\mathbf{u}_f}{\partial t} \right|_\mathrm{x} + \rho_{f} \left( \boldsymbol{u}_{f} \cdot \nabla_{\mathrm{x}} \right) \boldsymbol{u}_{f} - \nabla_{\mathrm{x}} \cdot \boldsymbol{\sigma}_{f} = \boldsymbol{f}^t_f , \quad \text{ in } \Omega^t_f \times \left[t_i,t_f \right]$
Mass conservation equation
$\nabla_{\mathrm{x}} \cdot \boldsymbol{u}_{f} = 0, \quad \text{ in } \Omega^t_f \times \left[t_i,t_f \right]$

we complete this set of equations with the fluid constitutive law

 $\boldsymbol{\sigma}_{f} = -p_f \boldsymbol{I} + 2\mu_f D(\boldsymbol{u}_{f})$

with strain tensor $D(\boldsymbol{u}_{f})$ defined by :

 $D(\boldsymbol{u}_{f}) = \frac{1}{2} (\nabla_\mathrm{x} \boldsymbol{u}_f + (\nabla_\mathrm{x} \boldsymbol{u}_f)^T)$

An alternative model is the Stokes model. It is valid in the case of small Reynolds number. It corresponds to the same formulation than Navier-Stokes equations but without the convective term $\left( \boldsymbol{u}_{f} \cdot \nabla_{\mathrm{x}} \right) \boldsymbol{u}_{f}$ .

## 3. CFD Toolbox

### 3.1. Models

The CFD Toolbox supports both the Stokes and the incompressible Navier-Stokes equations.

The fluid mechanics model (`Navier-Stokes` or `Stokes`) can be selected in json file:

Listing : select fluid model
``"Model": "Navier-Stokes"``

### 3.2. Materials

The next step is to define the fluid material by setting its properties namely the density $\rho_f$ and viscosity $\mu_f$. In next table, we find the correspondance between the mathematical names and the json names.

Table 1. Correspondance between fluid parameters and symbols in JSon files
Parameter Symbol

$\mu_f$

`mu`

$\rho_f$

`rho`

A `Materials` section is introduced in json file in order to configure the fluid properties. For each mesh marker, we can define the material properties associated.

Listing : Materials section
``````"Materials":
{
"<marker>"
{
"name":"water",
"rho":"1.0e3",
"mu":"1.0"
}
}``````

#### 3.2.1. Generalised Newtonian fluid

A non newtonian fluid is characterized by a non constant viscosity, which is a function of strain rate $\boldsymbol{D}\left(\boldsymbol{u}_{f}\right)$.

We start by introducing a metric of the rate of deformation, denoted by $\dot{\gamma}$:

 $\dot{\gamma} \equiv \sqrt{2 \ tr \left( \boldsymbol{D}\left(\boldsymbol{u}_{f}\right)^{2} \right) }$

We represent the viscosity $\mu_f$ as a function of $\dot{\gamma}$. The deviatoric stress tensor $\boldsymbol{\tau}$ is obtained thanks to generalised Newtonian model, which takes the following form:

 $\boldsymbol{\tau} = 2 \mu_f \left(\dot{\gamma} \right) \boldsymbol{D}\left(\boldsymbol{u}_{f}\right)$

The simplest example of a generalised Newtonian model is the power-law fluid, which has a viscosity given by:

 $\mu_f \left(\dot{\gamma} \right) = k \dot{\gamma}^{n-1}$

where $k$ and $n < 1$ are two parameters related to fluid properties.

Blood flow viscosity

In the context of blood flow modeling, an extension of the power model was proposed by Walburn and Schneck.

The parameters $k$ and $n$ are related to the hematocrit $Ht$ and Total Proteins Minus Albumin (TPMA) as follows

 $k = C_1 e^{C_2 Ht} e^{C_4 \text{TPMA} / Ht }, \quad\quad n = 1- C_3 H t$

and $C_i, i=1,..,4$ are parameters to fit with experimental data.

Another family of generalised Newtonian model can be defined from a function $\Phi$ express by:

 $\Phi\left( \dot{\gamma}, \mu_{\infty},\mu_{0} \right) = \frac{\mu\left(\dot{\gamma}\right) - \mu_{\infty}}{\mu_{0}-\mu_{\infty}}$

where $\mu_0$ and $\mu_{\infty}$ are the asymptotic viscosities at zero and infinite shear rate.

Viscosity law $\Phi\left( \dot{\gamma}, \mu_{\infty},\mu_{0} \right)$

Carreau

$\left(1+\left(\lambda\dot{\gamma}\right)^{2}\right)^{(n-1)/2}$

Carreau-Yasuda

$\left(1+\left(\lambda\dot{\gamma}\right)^{a}\right)^{(n-1)/a}$

The non Newtonian properties are defined in cfg file in fluid section.

The viscosity law is activated by:

Table 2. Viscosity law
option values

viscosity.law

newtonian, power_law, walburn-schneck_law, carreau_law, carreau-yasuda_law

Then, each model are configured with the options reported in the following table:

Viscosity law options unit

power_law

power_law.k

power_law.n

dimensionless

dimensionless

walburn-schneck_law

hematocrit

TPMA

walburn-schneck_law.C1

walburn-schneck_law.C2

walburn-schneck_law.C3

walburn-schneck_law.C4

Percentage

g/l

dimensionless

dimensionless

dimensionless

l/g

carreau_law

viscosity.zero_shear

viscosity.infinite_shear

carreau_law.lambda

carreau_law.n

$kg.m^{-1}.s^{-1}$

dimensionless

dimensionless

carreau-yasuda_law

viscosity.zero_shear

viscosity.infinite_shear

carreau-yasuda_law.lambda

carreau-yasuda_law.n

carreau-yasuda_law.a

$kg/(m \times s)$

$kg/(m \times s)$

dimensionless

dimensionless

dimensionless

### 3.3. Boundary Conditions

We start by a listing of boundary conditions supported in fluid mechanics model.

#### 3.3.1. Dirichlet on velocity

A Dirichlet condition on velocity field reads:

 $\boldsymbol{u}_f = \boldsymbol{g} \quad \text{ on } \Gamma$

or only a component of vector $\boldsymbol{u}_f =(u_f^1,u_f^2 ,u_f^3 )$

 $u_f^i = g \quad \text{ on } \Gamma$

Several methods are available to enforce the boundary condition:

• elimination

• Nitsche

• Lagrange multiplier

#### 3.3.2. Dirichlet on pressure

 $\begin{split} p & = g \\ \boldsymbol{u}_f \times {\boldsymbol{ n }} & = \boldsymbol{0} \end{split}$

#### 3.3.3. Neumann

Table 3. Neumann options
Name Expression

Neumann_scalar

$\boldsymbol{\sigma}_{f} \boldsymbol{n} = g \ \boldsymbol{n}$

Neumann_vectorial

$\boldsymbol{\sigma}_{f} \boldsymbol{n} = \boldsymbol{g}$

Neumann_tensor2

$\boldsymbol{\sigma}_{f} \boldsymbol{n} = g \ \boldsymbol{n}$

#### 3.3.4. Slip

 $\boldsymbol{u}_f \cdot \boldsymbol{ n } = 0$

#### 3.3.5. Inlet

The boundary condition at inlets allow to define a velocity profile on a set of marked faces $\Gamma_{\mathrm{inlet}}$ in fluid mesh:

 $\boldsymbol{u}_f = - g \ \boldsymbol{ n } \quad \text{ on } \Gamma_{\mathrm{inlet}}$

The function $g$ is computed from flow velocity profiles:

Constant profile
 $\text{Find } g \in C^0(\Gamma) \text{ such that } \\ \begin{eqnarray} g &=& \beta \quad &\text{ in } \Gamma \setminus \partial\Gamma \\ g&=&0 \quad &\text{ on } \partial\Gamma \end{eqnarray}$
Parabolic profile
 $\text{Find } g \in H^2(\Gamma) \text{ such that : } \\ \begin{eqnarray} \Delta g &=& \beta \quad &\text{ in } \Gamma \\ g&=&0 \quad &\text{ on } \partial\Gamma \end{eqnarray}$

where $\beta$ is a constant determined by adding a constraint to the inflow:

velocity_max

$\max( g ) = \alpha$

flow_rate

$\int_\Gamma ( g \ \boldsymbol{n} ) \cdot \boldsymbol{n} = \alpha$

Table 4. Inlet flow options
Option Value Default value Description

shape

`constant`,`parabolic`

select a shape profile for inflow

constraint

`velocity_max`,`flow_rate`

give a constraint wich controle velocity

expr

string

symbolic expression of constraint value

#### 3.3.6. Outlet flow

Table 5. Outlet flow options
Option Value Default value Description

model

free,windkessel

free

select an outlet modeling

##### Free outflow
 $\boldsymbol{\sigma}_{f} \boldsymbol{ n } = \boldsymbol{0}$
##### Windkessel model

We use a 3-element Windkessel model for modeling an outflow boundary condition. We define $P_l$ a pressure and $Q_l$ the flow rate. The outflow model is discribed by the following system of differential equations:

 \left\{ \begin{aligned} C_{d,l} \frac{\partial \pi_l}{\partial t} + \frac{\pi_l}{R_{d,l}} = Q_l \\ P_l = R_{p,l} Q_l + \pi_l \end{aligned} \right.

Coefficients $R_{p,l}$ and $R_{d,l}$ represent respectively the proximal and distal resistance. The constant $C_{d,l}$ is the capacitance of blood vessel. The unknowns $P_l$ and $\pi_l$ are called proximal pressure and distal pressure. Then we define the coupling between this outflow model and the fluid model by these two relationships:

 \begin{align} Q_l &= \int_{\Gamma_l} \boldsymbol{u}_f \cdot \boldsymbol{ n }_f \\ \boldsymbol{\sigma}_f \boldsymbol{ n }_f &= -P_l \boldsymbol{ n }_f \end{align}
Table 6. Windkessel options
Option Value Description

windkessel_coupling

explicit, implicit

coupling type with the Navier-Stokes equation

windkessel_Rd

real

distal resistance

windkessel_Rp

real

proximal resistance

windkessel_Cd

real

capacitance

#### 3.3.7. Implementation of boundary conditions in json

Boundary conditions are set in the json files in the category `BoundaryConditions`.

Then `<field>` and `<bc_type>` are chosen from type of boundary condition.

The parameter `<marker>` corresponds to mesh marker where the boundary condition is applied.

Finally, we define some specific options inside a marker.

Listing : boundary conditions in json
``````"BoundaryConditions":
{
"<field>":
{
"<bc_type>":
{
"<marker>":
{
"<option1>":"<value1>",
"<option2>":"<value2>",
// ...
}
}
}
}``````

#### 3.3.8. Options summary

Table 7. Boundary conditions
Field Name Option Entity

velocity

Dirichlet

expr

type

number

alemesh_bc

faces, edges, points

velocity_x

velocity_y

velocity_z

Dirichlet

expr

type

number

alemesh_bc

faces, edges, points

velocity

Neumann_scalar

expr

number

alemesh_bc

faces

velocity

Neumann_vectorial

expr

number

alemesh_bc

faces

velocity

Neumann_tensor2

expr

number

alemesh_bc

faces

velocity

slip

alemesh_bc

faces

pressure

Dirichlet

expr

number

alemesh_bc

faces

fluid

outlet

number

alemesh_bc

model

windkessel_coupling

windkessel_Rd

windkessel_Rp

windkessel_Cd

faces

fluid

inlet

expr

shape

constraint

number

alemesh_bc

faces

### 3.4. Body forces

Body forces are also defined in `BoundaryConditions` category in json file.

``````"VolumicForces":
{
"<marker>":
{
"expr":"{0,0,-gravityCst*7850}:gravityCst"
}
}``````

The marker corresponds to mesh elements marked with this tag. If the marker is an empty string, it corresponds to all elements of the mesh.

### 3.5. Post Processing

``````"PostProcess":
{
"Fields":["field1","field2",...],
"Measures":
{
"<measure type>":
{
"label":
{
"<range type>":"value",
"fields":["field1","field3"]
}
}
}
}``````
##### Exports for vizualisation

The fields allowed to be exported in the `Fields` section are:

• velocity

• pressure

• displacement

• vorticity

• stress or normal-stress

• wall-shear-stress

• density

• viscosity

• pid

• alemesh

##### Measures
• Points

• Force

• FlowRate

• Pressure

• VelocityDivergence

###### Points

In order to evaluate velocity or pressure at specific points and save the results in .csv file, the user must define:

• "<tag>" representing this data in the .csv file

• the coordinate of point

• the fields evaluated ("pressure" or "velocity")

``````"Points":
{
"<tag>":
{
"coord":"{0.6,0.2,0}",
"fields":"pressure"
},
"<tag>":
{
"coord":"{0.15,0.2,0}",
"fields":"velocity"
}
}``````
###### Flow rate

The flow rate can be evaluated and save on .csv file. The user must define:

• "<tag>" representing this data in the .csv file

• "<face_marker>" representing the name of marked face

• the fluid direction ("interior_normal" or "exterior_normal") of the flow rate.

``````"FlowRate":
{
"<tag>":
{
"markers":"<face_marker>",
"direction":"interior_normal"
},
"<tag>":
{
"markers":"<face_marker>",
"direction":"exterior_normal"
}
}``````
###### Forces

compute lift and drag

``"Forces":["fsi-wall","fluid-cylinder"]``
##### Export user functions

A function defined by a symbolic expression can be represented as a finite element field thanks to nodal projection. This function can be exported.

``````"Functions":
{
"toto":{ "expr":"x*y:x:y"},
"toto2":{ "expr":"0.5*ubar*x*y:x:y:ubar"},
"totoV":{ "expr":"{2*x,y}:x:y"}
},
"PostProcess":
{
"Fields":["velocity","pressure","pid","totoV","toto","toto2"],
}``````

### 3.6. Action

Let’s finish with a simple example in order to show how this works. We will interest us to a fluid flow into a cavity in 3D.

##### Feel++ code

Here is the code

First at all, we define our model type with

```typedef FeelModels::FluidMechanics< Simplex<FEELPP_DIM,1>,
Lagrange<OrderVelocity,Vectorial,Continuous,PointSetFekete>,
Lagrange<OrderPressure,Scalar,Continuous,PointSetFekete> > model_type;```

We choose here a $\mathbb{P}_2$ space for the velocity order and $\mathbb{P}_1$ space for the pressure order. This definition allows us to create our fluid model object FM like this

`auto FM = model_type::New("fluid");`

The method `New` retrieves all data from the configuration and json files and build a mesh if needed.

With this object, we can initialize our model parameters, such as velocity or boundaries conditions. Data on our model and on the numeric solver are then save and print on the terminal. This is made by

```FM->init();
FM->printAndSaveInfo();```

Now that our model is completed, we can solve the associated problem. To begin the resolution

`FM->isStationary()`

determine if our model is stationary or not.

If it is, then we need to solve our system only one time and export the obtained results.

```FM->solve();
FM->exportResults();```

If it’s not, our model is time reliant, and a loop on time is necessary. Our model is then solve and the results are export at each time step.

``` for ( ; !FM->timeStepBase()->isFinished(); FM->updateTimeStep() )
{
FM->solve();
FM->exportResults();
}```
###### Code
``{% include "../Examples/fluid_model.cpp" %}``
##### Configuration file

The config file is used to define options, linked to our case, we would have the possibility to change at will. It can be, for example, files paths as follows

```[fluid]
geofile=$cfgdir/cavity3d.geo filename=$cfgdir/cavity3d.json

[exporter]
directory=applications/models/fluid/cavity3d/fluid_tag``` It can also be resolution dependent parameters such as mesh elements size, methods used to define our problem and solvers. ```[fluid] solver=Oseen #Picard,Newton linearsystem-cst-update=false jacobian-linear-update=false snes-monitor=true snes-maxit=100 snes-maxit-reuse=100 snes-ksp-maxit=1000 snes-ksp-maxit-reuse=100 pc-type=lu #gasm,lu,fieldsplit,ilu``` In this case, we use Oseen to define our problem, we set the update of linear system constant and jacobian linear as "no update", we discretize values associated to SNES ( Scalable Nonlinear Equations Solvers ), and finally we choose LU as the preconditioner method. ###### Code ``{% include "../Examples/cavity3d.cfg" %}`` ##### Json file First at all, we define some general information like the name ( and short name ) and the model we would like to use ``````"Name": "Fluid Mechanics", "ShortName":"Fluid", "Model":"Navier-Stokes",`````` Then we define the material properties. In our case, the fluid, define by rho` its density in $kg\cdot m^{-3}$ and `mu` its dynamic viscosity in $kg\cdot (m \cdot s)^{-1}$, is the only material we have to define. ``````"Materials": { "Fluid":{ "name":"myFluidMat", "rho":"1.0", "mu":"0.01" } },`````` The boundary conditions are the next aspect we define. Here, we impose on the velocity $u_f$ Dirichlet conditions at two specific places : `lid` and `wall`. ``````"BoundaryConditions": { "velocity": { "Dirichlet": { "lid": { "expr":"{ 1,0,0}:x:y:z" }, "wall": { "expr":"{0,0,0}" } } } }`````` The post process aspect is the last one to define. We choose the fields we want to export ( velocity, pressure and pid ). Furthermore, we want to measure forces on `wall` and the pressure at point $A$. ``````"PostProcess": { "Fields":["velocity","pressure","pid"], "Measures": { "Forces":"wall", "Points": { "pointA": { "coord":"{0.5,0.5,0.5}", "fields":"pressure" } } } } }`````` ###### Code ``{% include "../Examples/cavity3d.json" %}`` ##### Compilation/Execution Once you’ve a build dir, you just have to realise the command `make` at `{buildir}/applications/models/fluid` This will generate executables named `feelpp_application_fluid_*`. To execute it, you need to give the path of the cfg file associated to your case, with `--config-file`. For example `./feelpp_application_fluid_3d --config-file={sourcedir}/applications/models/fluid/cavity/cavity3d.cfg` is how to execute the case ahead. The result files are then stored by default in ``` feel/applications/models/fluid/{case_name}/ {velocity_space}{pression_space}{Geometric_order}/{processor_used}``` If we return once again at our example, the result files are in ` feel/applications/models/fluid/cavity3d/P2P1G1/np_1` # Examples ## 4. Turek & Hron CFD Benchmark ### 4.1. Introduction We implement the benchmark proposed by Turek and Hron, on the behavior of drag and lift forces of a flow around an object composed by a pole and a bar, see Figure [img-geometry1]. The software and the numerical results were initially obtained from Vincent Chabannes.  This benchmark is linked to the Turek Hron CSM and Turek Hron FSI benchmarks. ### 4.2. Problem Description We consider a 2D model representative of a laminar incompressible flow around an obstacle. The flow domain, named $\Omega_f$, is contained into the rectangle $\lbrack 0,2.5 \rbrack \times \lbrack 0,0.41 \rbrack$. It is characterised, in particular, by its dynamic viscosity $\mu_f$ and by its density $\rho_f$. In this case, the fluid material we used is glycerine. Figure 1. Geometry of the Turek & Hron CFD Benchmark In order to describe the flow, the incompressible Navier-Stokes model is chosen for this case, define by the conservation of momentum equation and the conservation of mass equation. At them, we add the material constitutive equation, that help us to define $\boldsymbol{\sigma}_f$ The goal of this benchmark is to study the behavior of lift forces $F_L$ and drag forces $F_D$, with three different fluid dynamics applied on the obstacle, i.e on $\Gamma_{obst}$, we made rigid by setting specific structure parameters. To simulate these cases, different mean inflow velocities, and thus different Reynolds numbers, will be used. #### 4.2.1. Boundary conditions We set • on $\Gamma_{in}$, an inflow Dirichlet condition : $\boldsymbol{u}_f=(v_{in},0)$ • on $\Gamma_{wall}$ and $\Gamma_{obst}$, a homogeneous Dirichlet condition : $\boldsymbol{u}_f=\boldsymbol{0}$ • on $\Gamma_{out}$, a Neumann condition : $\boldsymbol{\sigma}_f\boldsymbol{ n }_f=\boldsymbol{0}$ #### 4.2.2. Initial conditions We use a parabolic velocity profile, in order to describe the flow inlet by $\Gamma_{in}$, which can be express by  $v_{cst} = 1.5 \bar{U} \frac{4}{0.1681} y \left(0.41-y\right)$ where $\bar{U}$ is the mean inflow velocity. However, we want to impose a progressive increase of this velocity profile. That’s why we define  v_{in} = \left\{ \begin{aligned} & v_{cst} \frac{1-\cos\left( \frac{\pi}{2} t \right) }{2} \quad & \text{ if } t < 2 \\ & v_{cst} \quad & \text{ otherwise } \end{aligned} \right. With t the time. Moreover, in this case, there is no source term, so $f_f\equiv 0$. ### 4.3. Inputs The following table displays the various fixed and variables parameters of this test-case. Table 8. Fixed and Variable Input Parameters Name Description Nominal Value Units $l$ elastic structure length $0.35$ $m$ $h$ elastic structure height $0.02$ $m$ $r$ cylinder radius $0.05$ $m$ $C$ cylinder center coordinates $(0.2,0.2)$ $m$ $\nu_f$ kinematic viscosity $1\times 10^{-3}$ $m^2/s$ $\mu_f$ dynamic viscosity $1$ $kg/(m \times s)$ $\rho_f$ density $1000$ $kg/m^3$ $f_f$ source term 0 $kg/(m^3 \times s)$ $\bar{U}$ characteristic inflow velocity CFD1 CFD2 CFD3 $0.2$ $1$ $2$ $m/s$ ### 4.4. Outputs As defined above, the goal of this benchmark is to measure the drag and lift forces, $F_D$ and $F_L$, to control the fluid solver behavior. They can be obtain from  $(F_D,F_L)=\int_{\Gamma_{obst}}\boldsymbol{\sigma}_f \boldsymbol{ n }_f$ where $\boldsymbol{n}_f$ the outer unit normal vector from $\partial \Omega_f$. ### 4.5. Discretization To realize these tests, we made the choice to used $P_N$-$P_{N-1}$ Taylor-Hood finite elements, described by Chabannes, to discretize space. With the time discretization, we use BDF, for Backward Differentation Formulation, schemes at different orders q. #### 4.5.1. Solvers Here are the different solvers ( linear and non-linear ) used during results acquisition.  type gmres relative tolerance 1e-13 max iteration 1000 reuse preconditioner false  relative tolerance 1e-8 steps tolerance 1e-8 max iteration CFD1/CFD2 : 100 | CFD3 : 50 max iteration with reuse CFD1/CFD2 : 100 | CFD3 : 50 reuse jacobian false reuse jacobian rebuild at first Newton step true  relative tolerance 1e-5 max iteration 1000 max iteration with reuse CFD1/CFD2 : 100 | CFD3 : 1000 reuse preconditioner false reuse preconditioner rebuild at first Newton step false  type lu package mumps ### 4.6. Running the model The configuration files are in `toolboxes/fluid/TurekHron`. The different cases are implemented in the corresponding `.cfg` files e.g. `cfd1.cfg`, `cfd2.cfg` and `cfd3.cfg`. The command line in feelpp-toolboxes docker reads Command line to execute CFD1 testcase `` mpirun -np 4 /usr/local/bin/feelpp_toolbox_fluid_2d --config-file cfd1.cfg``

The result files are then stored by default in

Results Directory
``feel/applications/models/fluid/TurekHron/"case_name"/"velocity_space""pression_space""Geometric_order"/"processor_used"``

For example, for CFD2 case executed on 12 processors, with a P_2 velocity approximation space, a P_1 pressure approximation space and a geometric order of 1, the path is

``feel/toolboxes/fluid/TurekHron/cfd2/P2P1G1/np_12``

### 4.7. Results

Here are results from the different cases studied in this benchmark.

#### 4.7.1. CFD1

Table 13. Results for CFD1
$\mathbf{N_{geo}}$ $\mathbf{N_{elt}}$ $\mathbf{N_{dof}}$ Drag Lift

Reference Turek and Hron

14.29

1.119

1

9874

45533 ($P_2/P_1$)

14.217

1.116

1

38094

173608 ($P_2/P_1$)

14.253

1.120

1

59586

270867 ($P_2/P_1$)

14.262

1.119

2

7026

78758 ($P_3/P_2$)

14.263

1.121

2

59650

660518 ($P_3/P_2$)

14.278

1.119

3

7026

146057 ($P_4/P_3$)

14.270

1.120

3

59650

1228831 ($P_4/P_3$)

14.280

1.119

All the files used for this case can be found in this rep [geo file, config file, json file]

#### 4.7.2. CFD2

Table 14. Results for CFD2
$\mathbf{N_{geo}}$ $\mathbf{N_{elt}}$ $\mathbf{N_{dof}}$ Drag Lift

Reference Turek and Hron

136.7

10.53

1

7020

32510 ($P_2/P_1$)

135.33

10.364

1

38094

173608 ($P_2/P_1$)

136.39

10.537

1

59586

270867 ($P_2/P_1$)

136.49

10.531

2

7026

78758 ($P_3/P_2$)

136.67

10.548

2

59650

660518 ($P_3/P_2$)

136.66

10.532

3

7026

146057 ($P_4/P_3$)

136.65

10.539

3

59650

1228831 ($P_4/P_3$)

136.66

10.533

All the files used for this case can be found in this rep [geo file, config file, json file]

#### 4.7.3. CFD3

As CFD3 is time-dependent ( from BDF use ), results will be expressed as

 $mean ± amplitude [frequency]$

where

• mean is the average of the min and max values at the last period of oscillations.

 $mean=\frac{1}{2}(max+min)$
• amplitude is the difference of the max and the min at the last oscillation.

 $amplitude=\frac{1}{2}(max-min)$
• frequency can be obtain by Fourier analysis on periodic data and retrieve the lowest frequency or by the following formula, if we know the period time T.

 $frequency=\frac{1}{T}$
Table 15. Results for CFD3
$\mathbf{\Delta t}$ $\mathbf{N_{geo}}$ $\mathbf{N_{elt}}$ $\mathbf{N_{dof}}$ $\mathbf{N_{bdf}}$ Drag Lift

0.005

Reference Turek and Hron

439.45 ± 5.6183[4.3956]

−11.893 ± 437.81[4.3956]

 0.01 1 8042 37514 ($P_2/P_1$) 2 437.47 ± 5.3750[4.3457] -9.786 ± 437.54[4.3457] 2 2334 26706 ($P_3/P_2$) 2 439.27 ± 5.1620[4.3457] -8.887 ± 429.06[4.3457] 2 7970 89790 ($P_2/P_2$) 2 439.56 ± 5.2335[4.3457] -11.719 ± 425.81[4.3457]
 0.005 1 3509 39843(P_3/P_2) 2 438.24 ± 5.5375[4.3945] -11.024 ± 433.90[4.3945] 1 8042 90582 ($P_3/P_2$) 2 439.25 ± 5.6130[4.3945] -10.988 ± 437.70[4.3945] 2 2334 26706 ($P_3/P_2$) 2 439.49 ± 5.5985[4.3945] -10.534 ± 441.02[4.3945] 2 7970 89790 ($P_3/P_2$) 2 439.71 ± 5.6410[4.3945] -11.375 ± 438.37[4.3945] 3 3499 73440 ($P_4/P_3$) 3 439.93 ± 5.8072[4.3945] -14.511 ± 440.96[4.3945] 4 2314 78168 ($P_5/P_4$) 2 439.66 ± 5.6412[4.3945] -11.329 ± 438.93[4.3945]
 0.002 2 7942 89482 (stem:[P_3/P_2) 2 439.81 ± 5.7370[4.3945] -13.730 ± 439.30[4.3945] 3 2340 49389 ($P_4/P_3$) 2 440.03 ± 5.7321[4.3945] -13.250 ± 439.64[4.3945] 3 2334 49266 ($P_4/P_3$) 3 440.06 ± 5.7773[4.3945] -14.092 ± 440.07[4.3945]

All the files used for this case can be found in this rep [geo file, config file, json file].

Figure 2. Lift and drag forces

### 4.8. Geometrical Order

 Add a section on geometrical order.

### 4.9. Conclusion

The reference results, Turek and Hron, have been obtained with a time step $\Delta t=0.05$. When we compare our results, with the same step and $\mathrm{BDF}_2$, we observe that they are in accordance with the reference results.

With a larger $\Delta t$, a discrepancy is observed, in particular for the drag force. It can also be seen at the same time step, with a higher order $\mathrm{BDF}_n$ ( e.g. $\mathrm{BDF}_3$ ). This suggests that the couple \Delta t=0.05 and $\mathrm{BDF}_2$ isn’t enough accurate.

### 4.10. Bibliography

References for this benchmark
• [TurekHron] S. Turek and J. Hron, Proposal for numerical benchmarking of fluid-structure interaction between an elastic object and laminar incompressible flow, Lecture Notes in Computational Science and Engineering, 2006.

• [Chabannes] Vincent Chabannes, Vers la simulation numérique des écoulements sanguins, Équations aux dérivées partielles [math.AP], Universitée de Grenoble, 2013.

## 5. Multifluid flows

We introduce here the multifluid flows benchmarks and the associated methdology.

### 5.1. Introduction

Let’s define a bounded domain $\Omega \subset \mathbb{R}^p$ ($p=2,3$) decomposed into two subdomains $\Omega_1$ and $\Omega_2$. We denote $\Gamma$ the interface between the two partitions. The goal of the level set method is to track implicitly the interface $\Gamma(t)$ moving at a velocity $\mathbf{u}$. The level set method has been described in [osher] and its main ingredient is a continuous scalar function $\phi$ (the /level set/ function) defined on the whole domain. This function is chosen to be positive in $\Omega_1$, negative in $\Omega_2$ and zero on $\Gamma$. The motion of the interface is then described by the advection of the level set function with a divergence free velocity field $\mathbf{u}$:

$\frac{\partial \phi}{\partial t} + \mathbf{u} \cdot \nabla \phi = 0,\quad \nabla \cdot \mathbf{u} = 0.$

A convenient choice for $\phi$ is a signed distance function to the interface. Indeed, the property $|\nabla \phi| = 1$ of distance functions eases the numerical solution and gives a convenient support for delta and Heaviside functions).

Nevertheless, it is known that the advection equation \eqref{eq:advection} does not conserve the property $|\nabla \phi|=1$. Thus, when $|\nabla \phi|$ is far from $1$ we have to reset $\phi$ as a distance function without moving the interface. To do so we can either use an Hamilton-Jacobi method or the fast marching method (see \cite{Winkelmann2007} for details about the fast marching method).

In two-fluid flow simulations, we need to define some quantities related to the interface such as the density, the viscosity, or some interface forces. To this end, we introduce the smoothed Heaviside and delta functions:

$H_{\varepsilon}(\phi) = \left\{ \begin{array}{cc} 0, & \phi \leq - \varepsilon,\\ \displaystyle\frac{1}{2} \left(1+\frac{\phi}{\varepsilon}+\frac{\sin(\frac{\pi \phi}{\varepsilon})}{\pi}\right), & -\varepsilon \leq \phi \leq \varepsilon, \\ 1, & \phi \geq \varepsilon. \end{array} \right.$
$\delta_{\varepsilon}(\phi) = \left\{ \begin{array}{cc} 0, & \phi \leq - \varepsilon,\\ \displaystyle\frac{1}{2 \varepsilon} \left(1+\cos(\frac{\pi \phi}{\varepsilon})\right), & -\varepsilon \leq \phi \leq \varepsilon, \\ 0, & \phi \geq \varepsilon. \end{array} \right.$

where $\varepsilon$ is a parameter defining a ``numerical thickness'' of the interface. A typical value of $\varepsilon$ is $1.5 h$ where $h$ is the mesh size of elements crossed by the iso-value $0$ of the level set function.

The Heaviside function is used to define parameters having different values on each subdomains. For example, we define the density of two-fluid flow as $\rho = \rho_2 + (\rho_1-\rho_2) H_{\varepsilon}(\phi)$ (we use a similar expression for the viscosity $\nu$). Regarding the delta function, it is used to define quantities on the interface. In particular, in the variational formulations, we replace integrals over the interface $\Gamma$ by integrals over the entire domain $\Omega$ using the smoothed delta function. If $\phi$ is a signed distance function, we have : $\int_{\Gamma} 1 \simeq \int_{\Omega} \delta_{\varepsilon}(\phi)$. If $\phi$ is not close enough to a distance function, then $\int_{\Gamma} 1 \simeq \int_{\Omega} |\nabla \phi| \delta_{\varepsilon}(\phi)$ which still tends to the measure of $\Gamma$ as $\varepsilon$ vanishes. However, if $\phi$ is not a distance function, the support of $\delta_{\varepsilon}$ can have a different size on each side of the interface. More precisely, the support of $\delta_{\varepsilon}$ is narrowed on the side where $|\nabla \phi|>1$ and enlarged on regions where $|\nabla \phi|<1$. It has been shown in [cottet] that replacing $\phi$ by $\frac{\phi}{|\nabla \phi|}$ has the property that $|\nabla \frac{\phi}{|\nabla \phi|}| \simeq 1$ near the interface and has the same iso-value $0$ as $\phi$. Thus, replacing $\phi$ by $\frac{\phi}{|\nabla \phi|}$ as support of the delta function does not move the interface. Moreover, the spread interface has the same size on each part of the level-set $\phi=0$. It reads $\int_{\Gamma} 1 \simeq \int_{\Omega} \delta_{\varepsilon}(\frac{\phi}{| \nabla \phi|})$. The same technique is used for the Heaviside function.

### 5.3. Numerical implementation and coupling with the fluid solver

We use the finite element C library <<Feel>> to discretize and solve the problem. Equation \eqref{eq:advection} is solved using a stabilized finite element method. We have implemented several stabilization methods such as Streamline Upwind Diffusion (SUPG), Galerkin Least Square (GLS) and Subgrid Scale (SGS). A general review of these methods is available in [Franca92]. Other available methods include the Continuous Interior Penalty method (CIP) are described in \cite{Burman2006}. The variational formulation at the semi-discrete level for the stabilized equation \eqref{eq:advection} reads, find $\phi_h \in {\mathbb R}_h^k$ such that $\forall \psi_h \in {\mathbb R}_h^k$ :

$\left(\int_{\Omega} \frac{\partial \phi_h}{\partial t} \psi_h + \int_{\Omega} (\mathbf{u}_h \cdot \nabla \phi_h) \psi_h\right) + S(\phi_h, \psi_h) = 0,$

where $S(\cdot, \cdot)$ stands for the stabilization bilinear form (see section \ref{sec:membr-inext} for description of ${\mathbb R}_h^k$ and $\mathbf{u}_h$). In our case, we use a BDF2 scheme which needs the solution at the two previous time step to compute the one at present time. For the first time step computation or after a reinitialization we use an Euler scheme.

### 5.4. Two-fluid flow

The two-fluid flow problem can be expressed by

\begin{align} \frac{D( \rho_\phi \boldsymbol{u} )}{Dt} - \boldsymbol{\nabla} \cdot ( 2 \mu_\phi \boldsymbol{D}({\boldsymbol{u}}) ) + \boldsymbol{\nabla} p = \boldsymbol{f}_\phi \\ \nabla \cdot \boldsymbol{u} = 0 \\ \partial_t \phi + \boldsymbol{u} \cdot \boldsymbol{\nabla} \phi =0 \end{align}

Where $\boldsymbol{f}_\phi$ is the force obtain by projection of the density of interfacial forces on the domain $\Omega$

$\boldsymbol{f}_{\phi} = \boldsymbol{g}(\phi, \boldsymbol{ n }, \kappa) \delta_\varepsilon(\phi)$

### 5.5. 2D Drops Benchmark

This benchmark has been proposed and realised by Hysing. It allows us to verify our level set code, our Navier-Stokes solver and how they couple together.

Computer codes, used for the acquisition of results, are from Vincent Doyeux, with the use of Chabannes's Navier-Stokes code.

#### 5.5.1. Problem Description

We want to simulate the rising of a 2D bubble in a Newtonian fluid. The bubble, made of a specific fluid, is placed into a second one, with a higher density. Like this, the bubble, due to its lowest density and by the action of gravity, rises.

The equations used to define fluid bubble rising in an other are the Navier-Stokes for the fluid and the advection one for the level set method. As for the bubble rising, two forces are defined :

• The gravity force : $\boldsymbol{f}_g=\rho_\phi\boldsymbol{g}$

• The surface tension force : $\boldsymbol{f}_{st}=\int_\Gamma\sigma\kappa\boldsymbol{ n }$

We denote $\Omega\times\rbrack0,3\rbrack$ the interest domain with $\Omega=(0,1)\times(0,2)$. $\Omega$ can be decompose into $\Omega_1$, the domain outside the bubble and $\Omega_2$ the domain inside the bubble and $\Gamma$ the interface between these two.

Figure 3. Geometry used in 2D Bubble Benchmark

Durig this benchmark, we will study two different cases : the first one with a ellipsoidal bubble and the second one with a squirted bubble.

##### Boundary conditions
• On the lateral walls, we imposed slip conditions

$\begin{eqnarray} \boldsymbol{u}\cdot\boldsymbol{n}&=&0 \\ t\cdot(\nabla\boldsymbol{u}+^t\nabla\boldsymbol{u})\cdot \boldsymbol{n}&=&0 \end{eqnarray}$
• On the horizontal walls, no slip conditions are imposed : $\boldsymbol{u}=0$

##### Initial conditions

In order to let the bubble rise, its density must be inferior to the density of the exterior fluid, so $\rho_1>\rho_2$

#### 5.5.2. Inputs

The following table displays the various fixed and variables parameters of this test-case.

Table 16. Fixed and Variable Input Parameters
Name Description Nominal Value Units

$\boldsymbol{g}$

gravity acceleration

$(0,0.98)$

$m/s^2$

$l$

length domain

$1$

$m$

$h$

height domain

$2$

$m$

$r$

$0.25$

$m$

$B_c$

bubble center

$(0.5,0.5)$

$m$

#### 5.5.3. Outputs

In the first place, the quantities we want to measure are $X_c$ the position of the center of the mass of the bubble, the velocity of the center of the mass $U_c$ and the circularity $c$, define as the ratio between the perimeter of a circle and the perimeter of the bubble. They can be expressed by

$\boldsymbol{X}_c = \dfrac{ \displaystyle \int_{\Omega_2} \boldsymbol{x}}{ \displaystyle \int_{\Omega_2} 1 } = \dfrac{ \displaystyle \int_\Omega \boldsymbol{x} (1-H_\varepsilon(\phi))}{ \displaystyle \int_\Omega (1-H_\varepsilon(\phi)) }$
$\boldsymbol{U}_c = \dfrac{\displaystyle \int_{\Omega_2} \boldsymbol{u}}{ \displaystyle \int_{\Omega_2} 1 } = \dfrac{\displaystyle \int_\Omega \boldsymbol{u} (1-H_\varepsilon(\phi))}{ \displaystyle \int_\Omega (1-H_\varepsilon(\phi)) }$
$c = \dfrac{\left(4 \pi \displaystyle \int_{\Omega_2} 1 \right)^{\frac{1}{2}}}{ \displaystyle \int_{\Gamma} 1} = \dfrac{ \left(4 \pi \displaystyle \int_{\Omega} (1 - H_\varepsilon(\phi)) \right) ^{\frac{1}{2}}}{ \displaystyle \int_{\Omega} \delta_\varepsilon(\phi)}$

After that, we interest us to quantitative points for comparison as $c_{min}$, the minimum of the circularity and $t_{c_{min}}$, the time needed to obtain this minimum, $u_{c_{max}}$ and $t_{u_{c_{max}}}$ the maximum velocity and the time to attain it, or $y_c(t=3)$ the position of the bubble at the final time step. We add a second maximum velocity $u_{max}$ and $u_{c_{max_2}}$ and its time $t_{u_{c_{max_2}}}$ for the second test on the squirted bubble.

#### 5.5.4. Discretization

This is the parameters associate to the two cases, which interest us here.

 Case $\rho_1$ $\rho_2$ $\mu_1$ $\mu_2$ $\sigma$ Re $E_0$ ellipsoidal bubble (1) 1000 100 10 1 24.5 35 10 squirted bubble (2) 1000 1 10 0.1 1.96 35 125

#### 5.5.6. Results

##### Test 2

We describe the different quantitative results for the two studied cases.

 h $c_{min}$ $t_{c_{min}}$ $u_{c_{max}}$ $t_{u_{c_{max}}}$ $y_c(t=3)$ lower bound 0.9011 1.8750 0.2417 0.9213 1.0799 upper bound 0.9013 1.9041 0.2421 0.9313 1.0817 0.02 0.8981 1.925 0.2400 0.9280 1.0787 0.01 0.8999 1.9 0.2410 0.9252 1.0812 0.00875 0.89998 1.9 0.2410 0.9259 1.0814 0.0075 0.9001 1.9 0.2412 0.9251 1.0812 0.00625 0.8981 1.9 0.2412 0.9248 1.0815
 h $c_{min}$ $t_{c_{min}}$ $u_{c_{max_1}}$ $t_{u_{c_{max_1}}}$ $u_{c_{max_2}}$ $t_{u_{c_{max_2}}}$ $y_c(t=3)$ lower bound 0.4647 2.4004 0.2502 0.7281 0.2393 1.9844 1.1249 upper bound 0.5869 3.0000 0.2524 0.7332 0.2440 2.0705 1.1380 0.02 0.4744 2.995 0.2464 0.7529 0.2207 1.8319 1.0810 0.01 0.4642 2.995 0.2493 0.7559 0.2315 1.8522 1.1012 0.00875 0.4629 2.995 0.2494 0.7565 0.2324 1.8622 1.1047 0.0075 0.4646 2.995 0.2495 0.7574 0.2333 1.8739 1.1111 0.00625 0.4616 2.995 0.2496 0.7574 0.2341 1.8828 1.1186

#### 5.5.7. Bibliography

References for this benchmark
• [Hysing] S. Hysing, S. Turek, D. Kuzmin, N. Parolini, E. Burman, S. Ganesan, and L. Tobiska, Quantitative benchmark computations of two-dimensional bubble dynamics, International Journal for Numerical Methods in Fluids, 2009.

• [Chabannes] V. Chabannes, Vers la simulation numérique des écoulements sanguins, Équations aux dérivées partielles. PhD thesis, Université de Grenoble, 2013.

• [Doyeux] V. Doyeux, Modélisation et simulation de systèmes multi-fluides, Application aux écoulements sanguins, PhD thesis, Université de Grenoble, 2014.

### 5.6. 3D Drop benchmark

The previous section described the strategy we used to track the interface. We couple it now to the Navier Stokes equation solver described in \cite{chabannes11:_high}. In the current section, we present a 3D extension of the 2D benchmark introduced in \cite{Hysing2009} and realised using Feel++ in \cite{Doyeux2012}.

#### 5.6.1. Benchmark problem

The benchmark objective is to simulate the rise of a 3D bubble in a Newtonian fluid. The equations solved are the incompressible Navier Stokes equations for the fluid and the advection for the level set:

$\begin{array}[lll] \rho\rho(\phi(\mathbf{x}) ) \left(\frac{\partial \mathbf{u}}{\partial t} + \mathbf{u} \cdot \nabla \mathbf{u} \right) + \nabla p - \nabla \cdot \left( \nu(\phi(\mathbf{x})) (\nabla \mathbf{u} + (\nabla \mathbf{u})^T) \right) &=& \rho ( \phi(\mathbf{x}) ) \mathbf{g}, \\ \nabla \cdot \mathbf{u} &=& 0, \\ \frac{\partial \phi}{\partial t} + \mathbf{u} \cdot \nabla \phi &=& 0, \end{array}$

where $\rho$ is the density of the fluid, $\nu$ its viscosity, and $\mathbf{g} \approx (0, 0.98)^T$ is the gravity acceleration.

The computational domain is $\Omega \times \rbrack0, T\rbrack$ where $\Omega$ is a cylinder which has a radius $R$ and a heigth $H$ so that $R=0.5$ and $H=2$ and $T=3$. We denote $\Omega_1$ the domain outside the bubble $\Omega_1= \{\mathbf{x} | \phi(\mathbf{x})>0 \}$, $\Omega_2$ the domain inside the bubble $\Omega_2 = \{\mathbf{x} | \phi(\mathbf{x})<0 \} stem:[ and stem:[\Gamma$ the interface $\Gamma = \{\mathbf{x} | \phi(\mathbf{x})=0 \}$. On the lateral walls and on the bottom walls, no-slip boundary conditions are imposed, i.e. $\mathbf{u} = 0$ and $\mathbf{t} \cdot (\nabla \mathbf{u} + (\nabla \mathbf{u})^T) \cdot \mathbf{n}=0$ where $\mathbf{n}$ is the unit normal to the interface and $\mathbf{t}$ the unit tangent. Neumann condition is imposed on the top wall i.e. $\dfrac{\partial \mathbf{u}}{\partial \mathbf{n}}=\mathbf{0}$. The initial bubble is circular with a radius $r_0 = 0.25$ and centered on the point $(0.5, 0.5, 0.)$. A surface tension force $\mathbf{f}_{st}$ is applied on $\Gamma$, it reads : $\mathbf{f}_{st} = \int_{\Gamma} \sigma \kappa \mathbf{n} \simeq \int_{\Omega} \sigma \kappa \mathbf{n} \delta_{\varepsilon}(\phi)$ where $\sigma$ stands for the surface tension between the two-fluids and $\kappa = \nabla \cdot (\frac{\nabla \mathbf{\phi}}{|\nabla \phi|})$ is the curvature of the interface. Note that the normal vector $\mathbf{n}$ is defined here as $\mathbf{n}=\frac{\nabla \phi}{|\nabla \phi|}$.

We denote with indices $1$ and $2$ the quantities relative to the fluid in respectively in $\Omega_1$ and $\Omega_2$. The parameters of the benchmark are $\rho_1$, $\rho_2$, $\nu_1$, $\nu_2$ and $\sigma$ and we define two dimensionless numbers: first, the Reynolds number which is the ratio between inertial and viscous terms and is defined as : $Re = \dfrac{\rho_1 \sqrt{|\mathbf{g}| (2r_0)^3}}{\nu_1}$; second, the E\"otv\"os number which represents the ratio between the gravity force and the surface tension $E_0 = \dfrac{4 \rho_1 |\mathbf{g}| r_0^2}{\sigma}$. The table below reports the values of the parameters used for two different test cases proposed in~\cite{Hysing2009}.

 Tests $\rho_1$ $\rho_2$ $\nu_1$ $\nu_2$ $\sigma$ Re $E_0$ Test 1 (ellipsoidal bubble) 1000 100 10 1 24.5 35 10 Test 2 (skirted bubble) 1000 1 10 0.1 1.96 35 125

The quantities measured in \cite{Hysing2009} are $\mathbf{X_c}$ the center of mass of the bubble, $\mathbf{U_c}$ its velocity and the circularity. For the 3D case we extend the circularity to the sphericity defined as the ratio between the surface of a sphere which has the same volume and the surface of the bubble which reads $\Psi(t) = \dfrac{4\pi\left(\dfrac{3}{4\pi} \int_{\Omega_2} 1 \right)^{\frac{2}{3}}}{\int_{\Gamma} 1}$.

#### 5.6.2. Simulations parameters

The simulations have been performed on the supercomputer SUPERMUC using 160 or 320 processors. The number of processors was chosen depending on the memory needed for the simulations. The table Numerical parameters used for the test 1 simulations summarize for the test 1 the different simulation properties and the table Mesh caracteristics give the carachteristics of each mesh.

 h Number of processors $\Delta t$ Time per iteration (s) Total Time (h) 0.025 360 0.0125 18.7 1.25 0.02 360 0.01 36.1 3.0 0.0175 180 0.00875 93.5 8.9 0.015 180 0.0075 163.1 18.4 0.0125 180 0.00625 339.7 45.3
 h Tetrahedra Points Order 1 Order 2 0.025 73010 14846 67770 1522578 0.02 121919 23291 128969 2928813 0.0175 154646 30338 187526 4468382 0.015 217344 41353 292548 6714918 0.0125 333527 59597 494484 11416557

The Navier-Stokes equations are linearized using the Newton’s method and we used a KSP method to solve the linear system. We use an Additive Schwarz Method for the preconditioning (GASM) and a LU method as a sub preconditionner. We run the simulations looking for solutions in finite element spaces spanned by Lagrange polynomials of order $(2,1,1)$ for respectively the velocity, the pressure and the level set.

#### 5.6.3. Results Test 1: Ellipsoidal bubble

Accordind to the 2D results we expect that the drop would became ellipsoid. The figure~\ref{subfig:elli_sh} shows the shape of the drop at the final time step. The contour is quite similar to the one we obtained in the two dimensions simulations. The shapes are similar and seems to converge when the mesh size is decreasing. The drop reaches a stationary circularity and its topology does not change. The velocity increases until it attains a constant value. Figure~\ref{subfig:elli_uc} shows the results we obtained with different mesh sizes.

#### 5.6.4. Bibliography

.

References for this benchmark
• [cottet]

• [Feelpp] C. Prud’homme et al.

• [osher] Osher1988, book_Sethian, book_Osher

• [Franca1992] Franca 1992