Dear All,

I am simulating a gas-solid two phase flow in a vertical pipe using Euler-Euler approach rather than Euler-Lagrange method. When I select solid as the thermodynamic state in the material editor, I have to use Euler-Lagrange method. However, I have to select liquid as the thermodynamic state if I want to use Euler-Euler approach. It's really a confusion since particles are solid. So, how to define solid phase in the materail editor?

Another problem is the boundary conditions. I noticed that in Tutorial 15 for air inlet, a velocity of 5m/s and zero volume fraction are used for water at air inlet. Why don't use 0m/s and zero volume fraction for water since there is no water entering into the domain through air inlet?

Liwau

Hi Liwau,

Both phases must be fluids (liquid or gas) for the Euler-Euler method. If you are modelling solid particles then your only option is the Lagrangian approach.

Glenn

Actually......

Just "tell" the model that the dispersed phase is a liquid. Give the material the appropriate density and a viscosity of nearly zero (1.0E-10). This is counter intuitive, but ensures that there is no visous transport of momentum within the solid phase. Make sure that you use Shiller Naumann for sphere's and set the disperse phase to laminar (otherwise your zero viscosity will be overridden by a turbulent viscosity).

Boundary conditions at inlets/outlets for phases which have zero volume fraction are best set to the continuous phase velocity. This ensures that the slip velocity between the phases is zero and the drag between phases will then be zero, even if numerical round-off gives you a trace component.

Jeff

HI name the thermodynamic phase of the solid as liquid and while specifying the morphologies of the fluid you can choose the option of dispersed solids. you can use very low solid viscosity of 1e-12. Note that you will not be able to use correct drag force models if you model the solid as dispersed liquid.

Dear Glenn, Jeff and friends,

I have a difficul task at hand (working from weeks still heading nowhere) and ur suggestions will be of great help. i am discussing this problem with CFX support engineers out here as well but not getting quite right.

I am trying to simulate a gas-liquid reaction in a packed bed (practically its a gas-solid reaction but as i cannot define varying comp solid in CFX, i m specifying it as liquid). Initially, reactor contatins 0.7 volume fraction of liquid (dispersed phase) and 0.3 volume fraction gas(continuous phase). Now through inlet, i m entering some air. air reacts with gasphase and liquidphase and produces some product. Now as per real physics, solid must not leave the system and also solid should not move in the system so in our case, liquid must not leave the system and volume fraction should remain constant.

i have run a few simulations but not getting quite right..

when i use degassing condition, liquid is not leaving the system but the volume fraction in the system is not fixed (its varying from 0 to 1) and also liquid is moving around.....

and when i specify avg static pressure at outlet, liquid is leaving the system !!!!!!!!!!!!!!

so neither case is satisfactory...Is there any way in which i can specify fixed velocity (ZERO in my case) for a particular phase in a multiphase simulation.

Can anybody comment on this how to resolve this problem. Is it possible in CFX 5.6 to fix velocity of a phase in multiphase simulation and solve momentum balance only for the other phase...

Eagerly waiting for some positive replys..

Thanks & Regards, Paresh Jain.