There are two .mfx files in the ZIP file you uploaded. I assume the real project is cobacoba.mfx and the air-reactor file is a stray.
The error you posted regarding DES_ETAT_FAC is a warning, not a fatal error. You can make this go away by setting a value for this key, but it should be OK to leave it at the default.
When I run the case, I get a different error:
In file '/opt/conda/conda-bld/mfix-solver_1676050431375/work/model/des/mpi_init_des_mod.f', around line 183: Error allocating 39293975568 bytes: Cannot allocate memory
Error termination. Backtrace:
#0 mpi_init_des_MOD_desmpi_init
at /usr/local/src/conda/mfix-solver-22.4.2/model/des/mpi_init_des_mod.f:182
#1 main_MOD_check_data
at /usr/local/src/conda/mfix-solver-22.4.2/model/main.f:698
#2 main_MOD_check_data
at /usr/local/src/conda/mfix-solver-22.4.2/model/main.f:580
#3 main_MOD_get_data
at /usr/local/src/conda/mfix-solver-22.4.2/model/main.f:562
#4 run_mfix
at /usr/local/src/conda/mfix-solver-22.4.2/model/mfix.f:127
#5 main_MOD_run_mfix0
at /usr/local/src/conda/mfix-solver-22.4.2/model/main.f:79
The primary issue is you have way too many particles for a DEM simulation and you run out of memory. That’s why it doesn’t run. Please take a look at existing tutorials to see examples of DEM simulations and how to set the geometry.
warning only like this…the simulation process is remaining Recovered: Dt… what is wrong? I try my best to check it again and again the set up but never got solution.
You should only include the interior wall of the geometry in the STL file. Here you have both sides.
You should orient the normal vectors so they point towards the fluid region. Here they point towards the solid region, so you are meshing the wall region, not the fluid region.
I like to have the STL geometry stick out from the inlet and outlet planes to get a better mesh along these planes.
You should always inspect the geometry/mesh before running the solver. This will most likely help you catch the issues above.
If you use incompressible gas, you may wan to increase the number of iterations for the Gas pressure equation (say 100, in the Numerics pane, Linear solver tab). You can also switch to ideal gas law, which may help with initial convergence.
sorry for the disturbance. i encountered similar problems with you, but i really don’t know how to include the interior wall only in stl file, could you please kindly share some experience with me?
Including only what I call the interior wall is the typical way we think of the geometry with CFD. We are modeling the fluid region, and this fluid region is bounded by boundaries along which we apply boundary conditions. The stl geometry defines these boundaries, i.e. surfaces where the fluid and solid are in contact. The STL geometry does not represent the solid volume around the fluid region. Imagine the solid is a mold and you pour wax into the mold. After the wax hardens, you have 2 objects: the mold and the wax object. The STL geometry should be that of the wax object, not the mold. The normal vectors should point towards the fluid region.
