Introduction
In this example, we check the correctness of SFEMaNS for a hydrodynamic problem with variable density and dynamical viscosity involving Dirichlet boundary conditions. The mass equation is not approximated. We consider a level set, solution of the same advection equation, that is used to reconstruct the density and the other fluid's properties.
We solve the level set equation:
\begin{align*} \partial_t \varphi + \bu \cdot \GRAD \varphi = f_\varphi. \end{align*}
We recontruct the density and dynamical viscosity as follows:
\begin{align*} \rho=\rho_1+(\rho_2\rho_1) F(\varphi), \\ \eta=\eta_1+(\eta_2\rho_1) F(\varphi), \end{align*}
with \(\eta_i\) and \(\rho_i\) data to define. The function \(F(\varphi)\) is either the identity (called linear reconstruction) or a piecewise polynomial function (called reg reconstruction).
We solve the NavierStokes equations with the momentum \(\bm=\rho\bu\) as dependent variable:
\begin{align*} \partial_t\bm + \DIV(\bm\otimes\bu)  \frac{2}{\Re} \DIV(\eta \epsilon(\bu)) +\GRAD p &=\bef, \\ \DIV \bu &= 0, \\ \bu_{\Gamma} &= \bu_{\text{bdy}} , \\ \bu_{t=0} &= \bu_0, \\ p_{t=0} &= p_0, \end{align*}
where \(\epsilon(\bu)=\frac{1}{2}(\GRAD \bu + \GRAD^s \bu)\) is the strain rate tensor.
These equations are solved in the domain \(\Omega= \{ (r,\theta,z) \in {R}^3 : (r,\theta,z) \in [0,1/2] \times [0,2\pi) \times [0,1]\} \) with \(\Gamma= \partial \Omega \). The data are the source terms \(f_\varphi\) and \(\bef\), the boundary data \(\bu_{\text{bdy}}\), the initial datas \(\bu_0\) and \(p_0\). The parameter \(\Re\) is the kinetic Reynolds number, the densities \(\rho_i\) and the dynamical viscosities \(\eta_i\).
Remarks:

The level set and the momentum equations can be stabilized with the entropy viscosity method used in test 15 (called LES).

For physical problem, the level set has to take values in [0,1] such that the interface is represented by \(\varphi^{1}(\{1/2\})\). The fluids area are respectively represented by \(\varphi^{1}(\{0\})\) and \(\varphi^{1}(\{1\})\). This test does not consider immiscible fluids. It involves manufactured solution with a smooth variable density. As a consequence, the level set does not take values in [0,1].

A compression term can also be added in the level set equation. This term allows the level set to remains sharp near the fluids interface represented by \( \varphi^{1}(\{1/2\}) \).
We refer to the section Extension to multiphase flow problem for more details on the algorithms implemented in SFEMaNS for multiphase problem.
Manufactured solutions
We approximate the following analytical solutions:
\begin{align*} u_r(r,\theta,z,t) &= 0, \\ u_{\theta}(r,\theta,z,t) &= r^2 \sin(z+t) , \\ u_z(r,\theta,z,t) &=0 , \\ p(r,\theta,z,t) &= 0, \\ \varphi(r,\theta,z,t) &=r^2+z^2, \\ \rho(r,\theta,z,t) &=1+r^2+z^2, \\ \eta(r,\theta,z,t) &=1+r^2+z^2. \end{align*}
where the source terms \(f_\varphi\), \(\bef\) and the boundary data \( \bu_{\text{bdy}}\) are computed accordingly.
Generation of the mesh
The finite element mesh used for this test is named Mesh_20_form.FEM
and has a mesh size of \(0.05\) for the P1 approximation. You can generate this mesh with the files in the following directory: ($SFEMaNS_MESH_GEN_DIR)/EXAMPLES/EXAMPLES_MANUFACTURED_SOLUTIONS/Mesh_20_form. The following image shows the mesh for P1 finite elements.
Finite element mesh (P1).

Information on the file condlim.f90
The initial conditions, boundary conditions and the forcing terms are set in the file condlim_test_25.f90
. Here is a description of the subroutines and functions of interest.

The subroutine
init_velocity_pressure
initializes the velocity field and the pressure at the time \(dt\) and \(0\) with \(dt\) being the time step. This is done by using the functions vv_exact and pp_exact as follows: time = 0.d0
DO i= 1, SIZE(list_mode)
mode = list_mode(i)
DO j = 1, 6
!===velocity
un_m1(:,j,i) = vv_exact(j,mesh_f%rr,mode,timedt)
un (:,j,i) = vv_exact(j,mesh_f%rr,mode,time)
END DO
DO j = 1, 2
!===pressure
pn_m2(:) = pp_exact(j,mesh_c%rr,mode,time2*dt)
pn_m1 (:,j,i) = pp_exact(j,mesh_c%rr,mode,timedt)
pn (:,j,i) = pp_exact(j,mesh_c%rr,mode,time)
phin_m1(:,j,i) = pn_m1(:,j,i)  pn_m2(:)
phin (:,j,i) = Pn (:,j,i)  pn_m1(:,j,i)
ENDDO
ENDDO

The function
init_level_set
initializes the level set at the time \(dt\) and \(0\) with \(dt\) being the time step. This is done by using the function level_set_exact as follows: time = 0.d0
DO i= 1, SIZE(list_mode)
mode = list_mode(i)
DO j = 1, 2
!===level_set
DO n = 1, inputs%nb_fluid 1
level_set_m1(n,:,j,i) = level_set_exact(n,j,vv_mesh%rr,mode,timedt)
level_set (n,:,j,i) = level_set_exact(n,j,vv_mesh%rr,mode,time)
END DO
END DO
END DO
We note there is one level set per interface and the different phases are stratified. So for nb_fluid fluids, we have inputs nb_fluid1 interfaces.

The function
vv_exact
contains the analytical velocity field. It is used to initialize the velocity field and to impose Dirichlet boundary conditions on the velocity field.

First we define the radial and vertical coordinates r, z.

We define the velocity field depending of its TYPE (1 and 2 for the component radial cosine and sine, 3 and 4 for the component azimuthal cosine and sine, 5 and 6 for the component vertical cosine and sine) as follows:
IF (m==0 .AND. TYPE==3) THEN
ELSE
vv = 0.d0
END IF
RETURN
where \(t\) is the time.

The function
pp_exact
contains the analytical pressure. It is used to initialize the pressure to zero.

The function level_set_exact
is used to initialize the level set.

We define the level set of the mode and its TYPE (1 for cosine and 2 for sine) as follows:
IF (interface_nb==1) THEN
IF (m==0 .AND. TYPE ==1) THEN
vv = rr(1,:)**2 + rr(2,:)**2
ELSE
vv = 0.d0
END IF

If more than one level set is considered, the computation is stopped.
ELSE
CALL error_petsc(' BUG in level_set_exact, we should compute only 1 level set')
END IF
RETURN
Indeed with two fluids there is one interface. So we should compute only one level set.

The function
source_in_NS_momentum
computes the source term \(\bef\) of the NavierStokes equations.

The function
source_in_level_set
computes the source term \(f_\varphi\) of the level set equations. It is equal to zero.
All the other subroutines present in the file condlim_test_25.f90
are not used in this test. We refer to the section Fortran file condlim.f90 for a description of all the subroutines of the condlim file.
Setting in the data file
We describe the data file of this test. It is called debug_data_test_25
and can be found in the following directory: ($SFEMaNS_DIR)/MHD_DATA_TEST_CONV_PETSC.

We use a formatted mesh by setting:
===Is mesh file formatted (true/false)?
.t.

The path and the name of the mesh are specified with the two following lines:
===Directory and name of mesh file
'.' 'Mesh_20_form.FEM'
where '.' refers to the directory where the data file is, meaning ($SFEMaNS_DIR)/MHD_DATA_TEST_CONV_PETSC.

We use four processor in the meridian section. It means the finite element mesh is subdivised in four.
===Number of processors in meridian section
4

We solve the problem for \(4\) Fourier modes.
===Number of Fourier modes
4

We use \(4\) processors in Fourier space.
===Number of processors in Fourier space
4
It means that each processors is solving the problem for \(4/4=1\) Fourier modes.

We do not select specific Fourier modes to solve.
===Select Fourier modes? (true/false)
As a consequence, the code approximates the problem on the first \(4\) Fourier modes.

We approximate the NavierStokes equations by setting:
===Problem type: (nst, mxw, mhd, fhd)
'nst'

We do not restart the computations from previous results.
===Restart on velocity (true/false)
.f.
It means the computation starts from the time \(t=0\).

We use a time step of \(0.005\) and solve the problem over \(200\) time iterations.
===Time step and number of time iterations
.005d0, 200

We do not apply mass correction on the level set.
===Do we apply mass correction? (true/false)
The default value is true.

We don't use a level set \(\varphi\) with values in \([0,1]\). So we do not kill the overshoot of the level set with respect of the interval \([0,1]\).
===Do we kill level set overshoot? (true/false)
The default value if false so these two lines are not required.

We set the number of domains and their label, see the files associated to the generation of the mesh, where the code approximates the NavierStokes equations.
===Number of subdomains in NavierStokes mesh
1
===List of subdomains for NavierStokes mesh
1

We set the number of boundaries with Dirichlet conditions on the velocity field and give their respective labels.
===How many
boundary pieces
for full Dirichlet BCs on velocity?
3
===List of
boundary pieces
for full Dirichlet BCs on velocity
2 4 5

We use the momentum as dependent variable for the NavierStokes equations.
===Solve NavierStokes with u (true) or m (false)?
If the density or the viscosity are variable, this parameter needs to be false. The default value is true (constant density and viscosity).

We use a BDF1 approximation of the time derivatives in the level set and momentum equations.
===Do we solve momentum with bdf2 (true/false)?
.f.
The default value is false.

We set the kinetic Reynolds number \(\Re\).

We use the entropy viscosity method to stabilize the level set equation.
===Use LES? (true/false)
.t.

We use the entropy viscosity method to stabilize the momentum equation.
==Use LES in momentum? (true/false)
.t.

We define the coefficient \(c_\text{e}\) of the entropy viscosity.
===Coefficient multiplying residual
.2d0

We give information on how to solve the matrix associated to the time marching of the velocity (or momentum in this case).

===Maximum number of iterations for velocity solver
100

===Relative tolerance for velocity solver
1.d6
===Absolute tolerance for velocity solver
1.d10

===Solver type for velocity (FGMRES, CG, ...)
GMRES
===Preconditionner type for velocity solver (HYPRE, JACOBI, MUMPS...)
MUMPS

We give information on how to solve the matrix associated to the time marching of the pressure.

===Maximum number of iterations for pressure solver
100

===Relative tolerance for pressure solver
1.d6
===Absolute tolerance for pressure solver
1.d10

===Solver type for pressure (FGMRES, CG, ...)
GMRES
===Preconditionner type for pressure solver (HYPRE, JACOBI, MUMPS...)
MUMPS

We give information on how to solve the mass matrix.

===Maximum number of iterations for mass matrix solver
100

===Relative tolerance for mass matrix solver
1.d6
===Absolute tolerance for mass matrix solver
1.d10

===Solver type for mass matrix (FGMRES, CG, ...)
CG
===Preconditionner type for mass matrix solver (HYPRE, JACOBI, MUMPS...)
MUMPS

We solve the level set equation.
===Is there a level set?
.t.

We want to consider one level set \(\varphi\), so we set: We note this test does not consider two immiscible fluids.

We do not use compression tools.
===Compression factor for level set
0.d0
This parameters is only relevant when we want to get sharp interface for immiscible fluids.

We define the parameters \((\rho_1,\rho_2)\) used to reconstruct the density.
===Density of fluid 0, fluid 1, ...
1.d0 2.d0

We define the parameters \((\eta_1,\eta_2)\) used to reconstruct the dynamical viscosity.
===Dynamic viscosity of fluid 0, fluid 1, ...
1.d0 2.d0

We define a multiplier coefficient.
===multiplier for h_min for level set
1.d0
This multiplier times the smallest mesh size is stored in the variable inputs%h_min_distance
. It can be used in the condlim file to set the wideness of the initial interface. It is not used in this case as the level set does not represent an interface between two immiscible fluids.

We use a linear reconstruction, meaning \(F(\varphi)=\varphi\).
===How are the variables reconstructed from the level set function? (lin, reg)
'lin'

We do not impose Dirichlet conditions on the level set.
===How many
boundary pieces
for Dirichlet BCs on level set?
0

We give information on how to solve the matrix associated to the time marching of the level set.

===Maximum number of iterations for level set solver
100

===Relative tolerance for level set solver
1.d6
===Absolute tolerance for level set solver
1.d10

===Solver type for level set (FGMRES, CG, ...)
GMRES
===Preconditionner type for level set solver (HYPRE, JACOBI, MUMPS...)
MUMPS

To get the total elapse time and the average time in loop minus initialization, we write:
===Verbose timing? (true/false)
.t.
These informations are written in the file lis
when you run the shell debug_SFEMaNS_template
.
Outputs and value of reference
The outputs of this test are computed with the file post_processing_debug.f90
that can be found in the following directory: ($SFEMaNS_DIR)/MHD_DATA_TEST_CONV_PETSC.
To check the well behavior of the code, we compute four quantities:

The L2 norm of the error on the velocity field.

The H1 norm of the error on the velocity field.

The L2 norm of the error on the level set.

The L2 norm of the error on the pressure.
These quantities are computed at the final time \(t=1\). They are compared to reference values to attest of the correctness of the code. These values of reference are in the last lines of the file debug_data_test_25
in the directory ($SFEMaNS_DIR)/MHD_DATA_TEST_CONV_PETSC. They are equal to:
============================================
(Mesh_10_form.FEM)
===Reference results
1.7489114810423408E004 L2 error on velocity
1.2910619903393045E003 H1 error on velocity
4.5642002105875500E003 L2 error on level set
1.3778684387869890E005 L2 error on pressure
To conclude this test, we show the profile of the approximated level set, density, pressure and velocity magnitude at the final time. These figures are done in the plane \(y=0\) which is the union of the half plane \(\theta=0\) and \(\theta=\pi\).
Level set in the plane plane y=0.

Density in the plane plane y=0.

Pressure in the plane plane y=0.

Velocity magnitude in the plane plane y=0.
