twoPhaseEulerFoam - test case validation
I'm working with the solver "twoPhaseEulerFoam", trying to reproduce the results shown in "Numerical simulation of the dynamic flowbehavior in a bubble column: A study of closures for turbulence and interface forces" by D. Zhang, N.G. Deen∗, J.A.M. Kuipers.
Did anyone already work on that topic ?
I have have test several parameters (mesh size, time step, void fraction at the inlet, lift force coefficient...) but so far I'm not able to reproduce the results in terms of the dispersed phase velocity and the continuous phase velocity.
If anyone is working on this, I'd be pleased to share any tips/work.
I followed the paper of Deen, Solberg and Hjertager of 2001 (Large eddy simulation of the Gas–Liquid ow in a square cross-sectioned bubble column)
There the same geometry is used. In order to do this simulations I had to extend the standard drag models (e.g. the Ishii-Zuber drag model) and I had to modify twoPhaseEulerFoam to make use of the generic turbulence models, in order to use LES turbulence. The k-eps turbulence model tends to establish a dominant vortex in the domain.
The mesh consists of 3 times 3 blocks. The top surface is modelled with a slip BC for the water. I had to set the inlet volume fraction to 0.6 in order to get a well behaving simulation. Consequenty, the inlet velocity has to be higher in order to match the volumetric gas flow rate.
The mesh fineness is limited by the Milelli condition. It says that the cell size should not be smaller than the bubble size. [A numerical analysis of confined turbulent bubble plumes, Massimo Milelli, PhD thesis, 2002]
One of the findings of Deen et al. was that the lift force is essential to match the measured profiles. My results also led me to that conclusion. In the attached images you see a case with drag, lift and virtual mass (case1) and a case with only drag as interfacial momentum exchange term (case4).
To initialize the simulation I run it with a fixed time step of 0.001 s for 10s, then I switch to variable time stepping and I activate the field averaging function object. Deen uses the averaged field values of the last 140s of the simulation. So, I ran the simulation for 140s after the initialisation.
Thank you for your answer.
I have a question regarding the use of LES in such cases. When the bubble's diameter is greater than 1 mm, considering the Milelli condition, does it make any sense for a LES computation ?
In the Zhang's publication I mentionned, they are working with bubbles of size of 0.004 meter in a square-section cylinder of 0.15x0.15 m² area. That seems to be really huge cells compared to the volume of fluid.
I am no expert on LES. However, using LES seems to work better than using kEpsilon.
The difference between VOF and Eulerian multiphase simulations is that in the Eulerian simulation you assume that the gas phase is dispersed in the liquid phase. If you further assume that your control volumes are larger than the bubbles you can treat the gas phase as a continuum. And that's were the Milelli condition comes in.
In VOF you want to resolve the surface that separates gas from liquid. That's why you need fine cells there.
That's all I can say besides, it works if you use LES.
Is there anyone out there who has done a horizontal channel/pipe test with twoPhaseEulerFoam? I am planning to use this solver for conditions where shear is important.
Setting LES CASE for bubble column
I am trying to simulate bubble column by using LES - twoPhaseEulerFoam in OF231. I am able to run the case for k-epsilon turbulence model but unable to do so for LES. Will you help me in setting case for LES?
|All times are GMT -4. The time now is 08:47.|