Representative Volume Element of Combustible Mixed Oxides for Nuclear Applications 

website: https://github.com/latug0/mfem-mgis-examples/tree/master/ex7

This example models a Representative Volume Element of a mixed oxide fuel under a uniform macroscopic strain. Its results are compared to the ones of Fauque et al. 2021 and Masson et al. 2020, who used an FFT method.

Problem solved 

Problem : RVE MOx 2 phases with elasto-viscoplastic behavior laws

Parameters :

start time = 0
end time = 5s
number of time step = 40

Imposed strain tensor :
        [ -a/2 ,   0  ,  0 ]
eps  =  [   0  , -a/2 ,  0 ] * t
        [   0  ,   0  ,  a ]
with a = 0.012 s^-1

Solver : HypreGMRES
Preconditioner : HypreBoomerAMG

Moduli and Norton behavior law parameters :
[ parameters       , matrix   , inclusions ]
[ Young Modulus    , 8.182e9  , 2*8.182e9  ];
[ Poisson Ratio    , 0.364    , 0.364      ];
[ Stress Threshold , 100.0e6  , 100.0e12   ];
[ Norton Exponent  , 3.333333 , 3.333333   ];
[ Temperature      , 293.15   , 293.15     ];

Element :
- Family H1
- Order 2

The matrix is the material 1 of the meshes. The inclusions are the material 2. Their stress threshold is high enough for them to remain elastic.

Illustration of a RVE with 634 spheres after 5 seconds.

Build the mesh 

Two meshes are provided in the mesh directory:

OneSphere.msh is the default mesh. Its spherical inclusion fills 17 % of the volume. Its elements are quadratic tetrahedra.
inclusion.msh contains one inclusion, which fills 11 % of the volume. Its elements are linear tetrahedra.

The meshes are generated with MEROPE and GMSH. MEROPE first generates a .geo file with the RSA algorithm. Its scripts are in the script_merope directory:

python3 script_17percent_minimal.py

GMSH then meshes the geometry. The .geo files are in the file_geo directory:

gmsh -3 OneSphere.geo

Run the simulation 

This command runs the default simulation from the build directory:

./mox2 --mesh mesh/OneSphere.msh

Available options 

Command line	Description	Default
`--mesh` or `-m`	Mesh file	mesh/OneSphere.msh
`--refinement` or `-r`	Number of uniform refinements of the mesh	0
`--nbsteps` or `-ns`	Number of time steps. The end time is 5 s.	40
`--order` or `-o`	Finite element order	2
`--verbosity-level` or `-v`	Verbosity level of the linear solvers	0
`--post-processing` or `-pp`, `--no-post-processing` or `-no-pp`	Export or not the results to Paraview	export
`--reference-file` or `-rf`	Reference values of the mean stresses in each material	no comparison
`--use-petsc` and `--petsc-configuration-file`	Use PETSc with the given configuration file. It requires MFEM built with PETSc.	no PETSc

Examples with other options:

./mox2 -r 2 -o 3 --mesh mesh/OneSphere.msh
mpirun -n 2 ./mox2 --use-petsc --petsc-configuration-file petscrc

Parallel computing mode 

The mesh with 634 spheres is not provided. These commands generate it and run the simulation in parallel:

gmsh -3 file_geo/634Spheres.geo
mpirun -n 12 ./mox2 --mesh file_geo/634Spheres.msh

On Topaze, a supercomputer of the CCRT, the commands are:

ccc_mprun -n 8 -c 1 -p milan ./mox2 -r 0 -o 3 --mesh mesh/OneSphere.msh
ccc_mprun -n 2048 -c 1 -p milan ./mox2 -r 2 -o 1 --mesh file_geo/634Spheres.msh

Test 

The test mox2 runs the default simulation. It compares the mean stresses in each material to the reference values computed with the same number of time steps:

40 time steps and OneSphere-avgStress-40steps.ref in the full test mode.
5 time steps and OneSphere-avgStress-5steps.ref in the restricted test mode. The average stress SZZ then differs by less than 9 % from the one computed with 40 time steps.

The test mox2-petsc does the same with PETSc. It requires MFEM built with PETSc.

Post-processing of simulation data 

The average stress SZZ is compared to the FFT results of Fauque et al. 2021 and Masson et al. 2020. These reference values are in results/res-fft.txt.

The MeanThermodynamicForces post-processing writes the file avgStress. It gives the mean stresses in each material as a function of time. The results of mfem-mgis are in the results directory:

res-mfem-mgis.txt gives the average stress SZZ over the RVE of OneSphere.msh at order 3. It is obtained with the awk command below.
res-mfem-mgis-634spheres-o2.txt is the avgStress file of the RVE with 634 spheres at order 2.

The RVE of OneSphere.msh contains 83 % of matrix and 17 % of inclusion. This awk command computes its average stress SZZ:

awk '{if(NR>13) print $1 " " 0.83*$4+0.17*$10}' avgStress > res-mfem-mgis.txt

The average stress SZZ at the end of the simulation, at t = 5 s, is:

Simulation	SZZ in MPa
FFT, `res-fft.txt`	93.05
`OneSphere.msh` at order 3, `res-mfem-mgis.txt`	94.63
`OneSphere.msh` at order 2, default	99.87
`OneSphere.msh` at order 1	140.0
634 spheres at order 2, `res-mfem-mgis-634spheres-o2.txt`	101.6

At order 1, the average stress is overestimated once the matrix flows. This is consistent with the volumetric locking of linear tetrahedra, since the viscoplastic flow is isochoric.

Display results with gnuplot 

gnuplot> plot "res-fft.txt" u 1:10 w l title "fft"
gnuplot> replot "res-mfem-mgis.txt" u 1:2 w l title "mfem-mgis"