Introduction
In this example, we check the correctness of SFEMaNS for a thermohydrodynamic problem. We use Dirichlet boundary conditions and a stabilization method called entropy viscosity that we refer as LES. We note this test does not involve manufactured solution and consist to check four quantities, like the kinetic energy of specific Fourier modes, are the same than the values of reference.
We solve the temperature equation:
\begin{align*} \partial_t T+ \bu \cdot \GRAD T  \kappa \LAP T &= 0, \\ T_{\Gamma} &= T_\text{bdy} , \\ T_{t=0} &= T_0, \end{align*}
and the NavierStokes equations:
\begin{align*} \partial_t\bu+\left(\ROT\bu\right)\CROSS\bu  \frac{1}{\Re}\LAP \bu +\GRAD p &= \DIV (\nu_E \GRAD \bu ) + \alpha T \textbf{e}_z, \\ \DIV \bu &= 0, \\ \bu_{\Gamma} &= \bu_{\text{bdy}} , \\ \bu_{t=0} &= \bu_0, \\ p_{t=0} &= p_0, \end{align*}
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 \(\Gamma= \partial \Omega\). We denote by \(\textbf{e}_z\) the unit vector in the vertical direction. The term \(\DIV (\nu_E \GRAD \bu )\) is a stabilization term that involve an artificial viscosity called the entropy viscosity. We refer to the section Entropy viscosity for under resolved computation for the definition of this term. The data are the boundary datas \(T_\text{bdy}\) and \(\bu_{\text{bdy}}\), the initial data \(T_0\), \(\bu_0\) and \(p_0\). The parameters are the thermal diffusivity \(\kappa\), the kinetic Reynolds number \(\Re\), the thermal gravity number \(\alpha\) and the real \(c_\text{e}\) for the entropy viscosity. We remind that these parameters are dimensionless.
Manufactured solutions
As mentionned earlier this test does not involve manufactured solutions. As consequence we do not consider specific source term and only initialize the variables to approximate.
\begin{align*} T(r,\theta,z,t=0) & = z  (z0.5)(z+0.5) \left(1+\cos(\theta)+\sin(\theta)+\cos(2\theta)+\sin(2\theta) \right) , \\ u_r(r,\theta,z,t=0) &= 0, \\ u_{\theta}(r,\theta,z,t=0) &= 0, \\ u_z(r,\theta,z,t=0) &=0, \\ p(r,\theta,z,t=0) &= 0, \end{align*}
The boundary datas \(T_\text{bdy}, \bu_{\text{bdy}}\) are computed accordingly.
Generation of the mesh
The finite element mesh used for this test is named RECT10_BENCHMARK_CONVECTION_LES.FEM
and has a mesh size of \(0.1\) for the P1 approximation. You can generate this mesh with the files in the following directory: ($SFEMaNS_MESH_GEN_DIR)/EXAMPLES/EXAMPLES_MANUFACTURED_SOLUTIONS/RECT10_BENCHMARK_CONVECTION_LES. 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 term in the NavierStokes equations are set in the file condlim_test_15.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. It 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 subroutine
init_temperature
initializes the temperature at the time \(dt\) and \(0\) with \(dt\) being the time step. It is done by using the function temperature_exact as follows: time = 0.d0
DO i= 1, SIZE(list_mode)
mode = list_mode(i)
DO j = 1, 2
tempn_m1(:,j,i) = temperature_exact(j, mesh%rr, mode, timedt)
tempn (:,j,i) = temperature_exact(j, mesh%rr, mode, time)
ENDDO
ENDDO

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. It is set to zero.

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

The function
temperature_exact
contains the analytical temperature. It is used to initialize the temperature and to impose Dirichlet boundary condition on the temperature.

We construct the radial and vertical coordinates r, z.

We set the temperature to zero.

For the Fourier mode \(m=0\) the temperature only depends of the TYPE 1 (cosine).
IF (m==0 .AND. TYPE==1) THEN
vv(:)= 
z  (
z5d1)*(
z+5d1)

For the Fourier mode \(m\geq1\), the temperature does not depend of the TYPE (1 for cosine and 2 for sine) and is defined as follows:
ELSE IF (m.GE.1) THEN
END IF
RETURN

The function
source_in_temperature
computes the source term denoted \(f_T\) in previous tests, of the temperature equation. As it is not used in this test, we set it to zero.

The function
source_in_NS_momentum
computes the source term \(\alpha T \textbf{e}_z\) of the NavierStokes equations 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 (TYPE==5) THEN
vv = inputs%gravity_coefficient*opt_tempn(:,1,i)
ELSE IF (TYPE==6) THEN
vv = inputs%gravity_coefficient*opt_tempn(:,2,i)
ELSE
vv = 0.d0
END IF
RETURN
All the other subroutines present in the file condlim_test_15.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_15
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
'.' 'RECT10_BENCHMARK_CONVECTION_LES.FEM'
where '.' refers to the directory where the data file is, meaning ($SFEMaNS_DIR)/MHD_DATA_TEST_CONV_PETSC.

We use one processor in the meridian section. It means the finite element mesh is not subdivised. To do so, we write:
===Number of processors in meridian section
1

We solve the problem for \(3\) Fourier modes.
===Number of Fourier modes
3

We use \(3\) processors in Fourier.
===Number of processors in Fourier space
3
It means that each processors is solving the problem for \(3/3=1\) Fourier modes.

We do not select specific Fourier modes to solve.
===Select Fourier modes? (true/false)

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.
===Restart on magnetic field (true/false)
.f.
It means the computation starts from the time \(t=0\).

We use a time step of \(0.05\) and solve the problem over \(10\) time iterations.
===Time step and number of time iterations
5.d2, 10

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?
2
===List of
boundary pieces
for full Dirichlet BCs on velocity
2 3

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

We use the entropy viscosity method to stabilize the equation.

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

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

===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 temperature equation (in the same domain than the NavierStokes equations).
===Is there a temperature field?
.t.

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

We set the thermal diffusivity \(\kappa\).
===Diffusivity coefficient for temperature (1:nb_dom_temp)
1.d0

We set the thermal gravity number \(\alpha\).
===Nondimensional gravity coefficient
50.d0

We set the number of boundaries with Dirichlet conditions on the temperature and give their respective labels.
===How many
boundary pieces
for Dirichlet BCs on temperature?
1
===List of
boundary pieces
for Dirichlet BCs on temperature
2

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

===Maximum number of iterations for temperature solver
100

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

===Solver type for temperature (FGMRES, CG, ...)
GMRES
===Preconditionner type for temperature 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)
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: ($SFEMaNS_DIR)/MHD_DATA_TEST_CONV_PETSC.
To check the well behavior of the code, we compute four quantities:

The kinetic energy of the Fourier mode \(m=0\).

The kinetic energy of the Fourier mode \(m=1\).

The kinetic energy of the Fourier mode \(m=2\).

The L2 norm of the velocity divergence divided by the L2 norm of the gradient of the velocity.
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_15
in the directory ($SFEMaNS_DIR)/MHD_DATA_TEST_CONV_PETSC. They are equal to:
============================================
RECT10_BENCHMARK_CONVECTION_LES.FEM, dt=5.d2, it_max=10
===Reference results
6.33685640432350423E004 !e_c_u_0
0.12910286398104689 !e_c_u_1
0.10838939329896366 !e_c_u_2
4.93403150219499723E002 !div(un)_L2/un_sH1
To conclude this test, we show the profile of the approximated, pressure, velocity magnitude and temperature at the final time. These figures are done in the plane \(y=0\) which is the union of the half plane \(\theta=0\) and \(\theta=\pi\).
Pressure in the plane plane y=0.

Velocity magnitude in the plane plane y=0.

Temperature in the plane plane y=0.
