Fluent 5/ASM : how to resolve the abnormality?
 

Using the ASM of the Fluent5 for water-sediment two-phase flows, the ultimate goal is to research the bed deformation, especially in the vicinity of the outlet--ideally a steady funneled-topography.However, observing the temporary result files, the velocites of both water and sediment are too large in the interior of the sediment region , in that they are the order of magnitude of the water's velocity in the pure water region, which is abnormal. Inevitably, all sediment would be disappeared. However, the steady funneled-topographyd has been obtained in the lab. experiments. How to avoid the abnormality that the velocities in the sediment region are too large, by means of the Fluent5/ASM ? Any suggestions would be appreciated!

Re: Fluent 5/ASM : how to resolve the abnormality?
 

Having "large" velocities points to lack of convergence or inappropriateness of the ASM model to your class of problem. Note that the Algebraic Slip Mixture model is not well suited to modelling sedimentation/settling.

Some points to look out for: 1. suspension must be dilute 2. small particle diameter (the particle relaxation time should be <0.01 s

An Eulerian formulation would better address the focus of your modelling => bed deformation

Re: Fluent 5/ASM : how to resolve the abnormality?
 

Lanre: Thanks for your response. The details as follows: 1 the ASM also is the Eulerian formulation 2 d50=0.36mm 3 and the boundary condition of the velocity_inlet has no sediment input, which guarantee the suspension is dilute. My goal just is focused on the bed deformation in the vicinity of the outlet. Somewhat, I have to agree with you that the Algebraic Slip Mixture model is not so well suited to modelling sedimentation/settling,such as my class of problem. Though, any tips would not be obtained as far as Fluent5/ASM is concerned? Best wishes,

Re: Fluent 5/ASM : how to resolve the abnormality?
 

The multi-fluid Eulerian-Eulerian models would address your sedimentation problem more realistically because four-way coupling: fluid-solid, solid-fluid, solid-solid, and fluid turbulence influenced by solids, would be addressed.

As for tips, try:

model as unsteady (initially use a timestep 1/10th of the characteristic flow time)

use the PISO algorithm

use body-force weighted discretization scheme for pressure

set URs to 1 (or 0.9 if not able to converge after 10-20 subiteration per time step). set UR for slip and vof to 0.2 and 0.5, respectively.

set operating pressure and location to be at the liquid surface

use implicit body force formulation

Re: Fluent 5/ASM : how to resolve the abnormality?
 

Lanre:

How are you getting along well with your researches? Thanks for your recommended tips, which have been followed. It is pity that the abnormality is what it was. I would have to further agree the Fluent 5/ASM is not suited to solve the bed deformation as my problems. More questions are:

(1) Whether the boundary condition for the outlet could be changed from OUTFLOW to PRESSURE_OUTLET? Because back-flow exists in the vicinity of the outlet, mainly near the water surface. In that case, how to define the pressure_outlet boundary condition?

(2) With the Non-equilibrium W.F. being better than the standard W.F., how to evaluate the mesh quality? My y-plus is (10-500) , and y-star is appropriate (0-70).

(3) It seems as if Fluent 5 couldn¡¯t deal with moving boundary. At the worst case, which commercial CFD software is suited well to bed deformation?

Thanks for your response, best regard,

eric