Hi
I work on my first coupling Project. I want to simulate a filter Receiver which separates the air from the conveyed material. The simulation I set up on the Ergun example. I use the same patches as in the example (inlet, outlet, wall). The problem is that always after a while the CFD solver crashes.
The courant max numbers are on the beginning below 0.4 (as Long as the solver is stable) and if I decrease the time step it only lasts longer until the CFD crashes.
The mesh I created in Salome and the "checkMesh" command Shows that the mesh is okay. There is also not a warning about non-orthogonal elements (and an increase of the non-orthogonal correctors dose not change the situation). Also a finer mesh does not solve the problem. I use a tet-mesh because I export the surface as an STL file to use them as walls in DEM.
If I use relaxationFactors (p=0.3, U=0.7, k=0.7...) than the simulation runs longer until it crashes (e.g. 5 s simulation time instead of 0.5). If I lower the relaxationFactors (p=0.05, U=0.2, k=0.2 ...) the simulation runs longer (e.g. 15 s simulation time).
If I increase the viscosity (from 1.5e-4 to 1.5e-2) it seems to be stable over the simulation time of 20 s.
I run pure CFD simulations and there are the same effects so it does not seem to be a coupling problem.
When I run steady state simulations (simpleFoam) it converges. I also try to use the U and p field as initial fields for the transient simulation (pisoFoam) but also than the simulation crashes after a while.
So what can I do to improve the stability of the solver? What is missing or wrong? Thanks for evry suggestion.
cgoniva | Wed, 04/02/2014 - 09:38
Hello Urs,
Hello Urs,
using very fine meshes (in the order of the particle size) can lead to problems as the exchange fields become inhomogeneous. Further tet meshes in general are not too good for OpenFOAM's solvers.
Try switchin off turbulence to see if something is wrong with these settings.
Hope That helps?
Cheers, Chris
uhelfenstein | Wed, 04/02/2014 - 10:34
Hi Chris,
Hi Chris,
Thank you for the answer.
What does it mean a fine mesh. Is a fine mesh if the element size is smaller than the particle size? Which ratio is recommended to use?
I use a corser mesh and that improves the stability.
I uses tet-meshes because I ned the surface of the mesh for DEM walls. Is there an other possibility or use different meshes for DEM and CFD?
Regards,
Urs
alice | Wed, 04/16/2014 - 10:32
Hi Urs,
Hi Urs,
generally one should make sure that the particles are smaller than the fluid cells in unresolved CFD-DEM. Particles that cover a whole cell or even a number of cells are problematic.
Using different meshes for CFD and DEM is no problem. If you have an OpenFOAM mesh you can use the command surfaceMeshTriangulate to create an according stl-mesh. The command comes with OpenFOAM, a brief documentation is provided.
Cheers,
Alice
uhelfenstein | Thu, 04/17/2014 - 10:54
[solved] Simulation now stable
Hi Alice,
Thanks for your input. To increase the mesh size was a big step towards a stable simulation. By refining the mesh I was going into the wrong direction. Another point was to lower the relaxation factor of the U solver because the unstability starts always by an increasing of the residuals of the U solver.
I also run a steady state simulation (simpleFoam) and use the results of the fields as Initial condition for the transient siumlation (pisoFoam).
So now the simulation runs stable.
Thank you also for the hint about the OpenFOAM command surfaceMeshTriangle. I will try this.
Regards,
Urs