SFEMaNS  version 4.1 (work in progress) Reference documentation for SFEMaNS
Test 2: Navier-Stokes periodic

### Introduction

In this example, we check the correctness of SFEMaNS for a hydrodynamic problem involving periodic and Dirichlet boundary conditions.

We solve the Navier-Stokes equations:

\begin{align*} \partial_t\bu+\left(\ROT\bu\right)\CROSS\bu - \frac{1}{\Re}\LAP \bu +\GRAD p &=\bef, \\ \DIV \bu &= 0, \\ \bu_{|\{z=0\}} &= \bu_{|\{z=1\}} , \\ p_{|\{z=0\}} &= p_{|\{z=1\}} , \\ \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 $$\Gamma= \partial \Omega\setminus\{ \{z=0\} \cup \{z=1\} \}$$. The data are the source term $$\bef$$, the boundary data $$\bu_{\text{bdy}}$$, the initial data $$\bu_0$$ and $$p_0$$. The parameter $$\Re$$ is the kinetic Reynolds number.

### Manufactured solutions

We approximate the following analytical solutions:

\begin{align*} u_r(r,\theta,z,t) &= -r^2 \left( 1-2\pi r \sin(2\pi z) \right) \sin(\theta) \cos(t), \\ u_{\theta}(r,\theta,z,t) &= -3 r^2 \cos(\theta) \cos(t), \\ u_z(r,\theta,z,t) &= r^2 \left( 4\cos(2\pi z) +1 \right) \sin(\theta) \cos(t), \\ p(r,\theta,z,t) &= r^2 \cos(2\pi z)\cos(\theta)\cos(t), \end{align*}

where the source term $$\bef$$ and the boundary data $$\bu_{\text{bdy}}$$ are computed accordingly.

The finite element mesh used for this test is named Mesh_10_form.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/Mesh_10_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 term $$\textbf{f}$$ in the Navier-Stokes equations are set in the file condlim_test_2.f90. Here is a description of the subroutines and functions of interest. 1. 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,time-dt) 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,time-2*dt) pn_m1 (:,j,i) = pp_exact(j,mesh_c%rr,mode,time-dt) 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 2. 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. 1. First we define $$2\pi$$ as follows: k = 2*ACOS(-1.d0) 2. We define the radial and vertical coordinates r, z. r = rr(1,:) z = rr(2,:) 3. If the Fourier mode m is not equal to 1, the velocity field is set to zero. IF (m/=1) THEN vv = 0.d0 RETURN END IF 4. For the Fourier mode $$m=1$$, 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 (TYPE == 1) THEN vv(:) = 0.d0 ELSEIF (TYPE == 2 .AND. m /= 0) THEN vv(:) = -r**2*(1-k*r*SIN(k*z)) ELSEIF (TYPE == 3) THEN vv(:) = -3*r**2 ELSEIF (TYPE == 4 .AND. m /= 0) THEN vv(:) = 0.d0 ELSEIF (TYPE == 5) THEN vv(:) = 0.d0 ELSEIF (TYPE == 6 .AND. m /= 0) THEN vv(:) = r**2*(4*COS(k*z)+1) ENDIF vv(:) = vv(:) * COS(t) RETURN where $$t$$ is the time. The reader can note that the condition "m /= 0" is not needed since we already set vv to zero when we are not dealing with the Fourier mode $$m=1$$. 3. The function pp_exact contains the analytical pressure. It is used to initialize the pressure. 1. First we define the real $$2\pi$$. k = 2*ACOS(-1.d0) 2. If the Fourier mode m, is not equal to 1, the pressure is set to zero. IF (m/=1) THEN vv = 0.d0 RETURN END IF 3. For the Fourier mode $$m=1$$, the pressure only depends of the TYPE 1 (cosine) so we write: IF (TYPE==1) THEN vv(:)= rr(1,:)**2*COS(k*rr(2,:))*COS(t) ELSE vv(:) = 0.d0 END IF RETURN where $$t$$ is the time. Thus the coefficient in sine of the presure for the Fourier mode $$1$$ is zero. 4. The function source_in_NS_momentum computes the source term $$\bef$$ of the Navier-Stokes equations. All the other subroutines present in the file condlim_test_2.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_2 and can be found in the following directory: ($SFEMaNS_DIR)/MHD_DATA_TEST_CONV_PETSC.

1. We use a formatted mesh by setting:
===Is mesh file formatted (true/false)?
.t.
2. The path and the name of the mesh are specified with the two following lines:
===Directory and name of mesh file
'.' 'Mesh_10_form.FEM'
where '.' refers to the directory where the data file is, meaning ($SFEMaNS_DIR)/MHD_DATA_TEST_CONV_PETSC. 3. We use two processors in the meridian section. It means the finite element mesh is subdivised in two. ===Number of processors in meridian section 2 4. We solve the problem for $$3$$ Fourier modes. ===Number of Fourier modes 3 5. We use $$3$$ processors in Fourier space. ===Number of processors in Fourier space 3 It means that each processors is solving the problem for $$3/3=1$$ Fourier modes. 6. We select specific Fourier modes to solve by setting: ===Select Fourier modes? (true/false) .t. 7. We give the list of the Fourier modes to solve. ===List of Fourier modes (if select_mode=.TRUE.) 0 1 2 We note that setting select Fourier modes to false would give the same result as we select the first three Fourier modes. 8. We approximate the Navier-Stokes equations by setting: ===Problem type: (nst, mxw, mhd, fhd) 'nst' 9. We do not restart the computations from previous results. ===Restart on velocity (true/false) .f. It means the computation starts from the time $$t=0$$. 10. We use a time step of $$0.01$$ and solve the problem over $$100$$ time iterations. ===Time step and number of time iterations .01d0, 100 11. We set periodic boundary condition. 1. We set the number of pair of boundaries that has to be periodic. ===How many pieces of periodic boundary? 1 2. We give the label of the boundaries and the vector that lead to the first boundary to the second one. ===Indices of periodic boundaries and corresponding vectors 4 2 .0d0 1.d0 We note that we need as much as lines as the number of pairs of boundaries with periodic condition. 12. We set the number of domains and their label, see the files associated to the generation of the mesh, where the code approximates the Navier-Stokes equations. ===Number of subdomains in Navier-Stokes mesh 1 ===List of subdomains for Navier-Stokes mesh 1 13. 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? 1 ===List of boundary pieces for full Dirichlet BCs on velocity 5 14. We set the kinetic Reynolds number $$\Re$$. ===Reynolds number 1.d0 15. We do not apply penalty on the divergence of the velocity field. ===Coefficient for penalty of divergence in NS? 0.d0 We note $$0$$ is the defaut value so this two lines are not required. 16. We give information on how to solve the matrix associated to the time marching of the velocity. 1. ===Maximum number of iterations for velocity solver 100 2. ===Relative tolerance for velocity solver 1.d-6 ===Absolute tolerance for velocity solver 1.d-10 3. ===Solver type for velocity (FGMRES, CG, ...) GMRES ===Preconditionner type for velocity solver (HYPRE, JACOBI, MUMPS...) MUMPS 17. We give information on how to solve the matrix associated to the time marching of the pressure. 1. ===Maximum number of iterations for pressure solver 100 2. ===Relative tolerance for pressure solver 1.d-6 ===Absolute tolerance for pressure solver 1.d-10 3. ===Solver type for pressure (FGMRES, CG, ...) GMRES ===Preconditionner type for pressure solver (HYPRE, JACOBI, MUMPS...) MUMPS 18. We give information on how to solve the mass matrix. 1. ===Maximum number of iterations for mass matrix solver 100 2. ===Relative tolerance for mass matrix solver 1.d-6 ===Absolute tolerance for mass matrix solver 1.d-10 3. ===Solver type for mass matrix (FGMRES, CG, ...) CG ===Preconditionner type for mass matrix solver (HYPRE, JACOBI, MUMPS...) MUMPS ### 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:

1. The L2 norm of the error on the velocity field.
2. The H1 norm of the error on the velocity field.
3. The L2 norm of the divergence of the velocity field.
4. 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_2 in the directory(\$SFEMaNS_DIR)/MHD_DATA_TEST_CONV_PETSC. They are equal to:

============================================
(Mesh_10_form.FEM)
===Reference results
9.010064775995388E-005 L2 error on velocity
4.268199030547359E-003 H1 error on velocity
2.016626738178190E-002 L2 norm of divergence
2.993344602551886E-003 L2 error on pressure

To conclude this test, we show the profile of the approximated 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 $$\theta=\pi$$.

 Pressure in the plane plane y=0. Velocity magnitude in the plane plane y=0.