I’ve already tried increasing it to 150 but it still doesn’t work so I need to keep increasing it? When the small cell tolerance or snap tolerance is very small, the particles will disappear but they will disappear very little. But when increasing the small cell tolerance or snap tolerance, the particles disappear in very large amounts. So you still think it is a solid time step problem? I will try to keep increasing the solid time step (Tcoll/Dt_solid>150). Finally I would like to know if you have adjusted the parameters related to mesh generation in Mesher? Would it be possible for you to share the case where no backflow occurred? Thanks again Jeff for your reply and have a great day!
Please see attached a case that ran to completion without backflow. The issue with particles leaving the domain is that there is a small gap between the stl geometry and the cut cell cut face (due to the curvature of the geoemtry. This is usually not a problem but the particles are smaller than that gap so they are flagged as roghe particles and are deleted. Using a relatively fine mesh helps.
(Particle size artificially increased during postprocessing foe better visibility)
Thank you very much Jeff! This solves a problem that has been bothering me for a long time. I would also like to ask why the DES grid is set so thin?
I just set it up that way while troubleshooting. This is actually fairly coarse based on your particle size. The default value is a des grid spacing equal to 3 times the largest particle diameter, which is 577x1531x577 here. My guess is you want to eventually run the simulation with more than 200 particles so you may need to go finer than my setting.
Thanks Jeff for your reply. I’ve never quite understood what the purpose of the DES mesh is? As I understand it, if the IMAX is smaller, it indicates that the coarser the DES mesh is, the more particles need to be searched? Or to put it another way, what determines the extent to which particles search their neighbors?
Yes the des grid is used to build a list of neighbor particles. For a given particle size, the coarser it is (low DESGRIDSEARCH_IMAX), the more particles will be in a desgrid cell and the more potential neighbors a particle will have, which will slow down the computation when checking for particle collision.
Thank you very much for your reply, Jeff. It was very helpful! I have one last question, the turbulence model still doesn’t converge even though I adjusted the value of ε a lot. For example, k=6 and ε=500,2000,5000,10000.
check_cell_movement.f (17.0 KB)
The divergence is due to the presence of small cut cells, and I set the small cut cell to zero to avoid particle leakage.
Please try with the attached (copy to project directory and rebuild the solver), and set a small value for the small cut cell tolerance (say 0.005 or 0.01) so it converges. The attached file will not delete particles that are in small cut cells. Not sure if this will work but it is worth trying.
I am not sure about what values you should use for k and epsilon at the IC and BC, others can chime in.
Thank you very much Jeff for your answer, I tried it but it didn’t seem to work.
But when I commented out ‘CALL CHECK_CELL_MOVEMENT’ on line 189 in the particles_in_cell.f file, the particles don’t seem to disappear. But this requires turning off ‘re-indexing of cell’. If you don’t turn it off, an error will occur, as shown in the second picture. And if you turn off ‘re-indexing of cell’, it will slow down the calculation greatly. I would like to know if there are other codes that can be changed.
You mean you increased the small cell tolerance (to what value?) and it is converging, but particles leak out?
I first tested if the particles would leak out and did not turn on the turbulence model. When I increased the small cell tolerance to 0.01, the particles leaked out (the particles were 50 microns in diameter).
Can you try with the original 150 microns to see if we are making progress? Going down to 50 microns bring another level of complexity for DEM.
Hi Jeff. I tried it, and it seems to work. When using small particle sizes, the solid time step must be reduced. However, I still cannot get the turbulence model to converge.
Hi, Jeff. I tried the MIXING_LENGTH turbulence model and set ic_l_scale=0.0001, and it works. Does any developer know how to make the k-ε turbulence model converge?
Did you try to set a low value for the max turbulent viscosity?
Hi, Jeff. I tried settings of max turbulent viscosity = 10, 100, 500, and 1000, but all of them failed 
.
I tried 0.01 and 0.1, this seems to converge.
It works! I didn’t expect it to need to be scaled down so much! Thank you very much, Jeff. I would like to know if MFIX can use the stabilised flow field as the initialised flow field. That is, can the flow field after the pure fluid simulation has converged be used in MFIX-DEM?