[fabfi]

Dear all,

I got trouble with a transient multiphase case (continueous domains). It includes

- air (top)
- cold water (middle) separated through a narrow gap from
- hot water (bottom)

air and water are different domains with a free surface in between.

The hot water should mix up with the cold water and then heat up the air (there is also CHT around, but not interesting for the specific problem). Buoyancy is activated.

With a closed volume everything is working fine but I do not want to cool down the hot water (represents a big domain where temperature change is negligible). Thus, I defined an opening at the bottom. The opening relative pressure is zero and the temperature is equal to the hot water temperature. Now, hot water flows back in and temperature stays constant.

BUT the interface between air and cold water domain moves down, means the water level decreases. Of course, gravity does his job. Is there any trick to avoid this or can anyone recommend another workaround?

[fabfi]

  BOUNDARY: Opening
       Boundary Type = OPENING
       Interface Boundary = Off
       Location = F1049.1034
       BOUNDARY CONDITIONS: 
         FLOW DIRECTION: 
           Option = Normal to Boundary Condition
         END
         FLOW REGIME: 
           Option = Subsonic
         END
         HEAT TRANSFER: 
           Opening Temperature = 98 [K]
           Option = Opening Temperature
         END
         MASS AND MOMENTUM: 
           Option = Opening Pressure and Direction
           Relative Pressure = 0 [Pa]
         END
       END
       FLUID: Steam
         BOUNDARY CONDITIONS: 
           VOLUME FRACTION: 
             Option = Value
             Volume Fraction = 0
           END
         END
       END
       FLUID: Water
         BOUNDARY CONDITIONS: 
           VOLUME FRACTION: 
             Option = Value
             Volume Fraction = 1
           END
         END
       END
     END
     DOMAIN MODELS: 
       BUOYANCY MODEL: 
         Buoyancy Reference Density = 1 [kg m^-3]
         Gravity X Component = 0 [m s^-2]
         Gravity Y Component = -9.81 [m s^-2]
         Gravity Z Component = 0 [m s^-2]
         Option = Buoyant
         BUOYANCY REFERENCE LOCATION: 
           Option = Automatic
         END
       END
       REFERENCE PRESSURE: 
         Reference Pressure = 1 [atm]
       END
     END
     FLUID DEFINITION: Steam
       Material = Air Ideal Gas
       Option = Material Library
       MORPHOLOGY: 
         Option = Continuous Fluid
       END
     END
     FLUID DEFINITION: Water
       Material = Water
       Option = Material Library
       MORPHOLOGY: 
         Option = Continuous Fluid
       END
     END
       FLUID: Steam
         FLUID BUOYANCY MODEL: 
           Option = Density Difference
         END
       END
       FLUID: Water
         FLUID BUOYANCY MODEL: 
           Option = Density Difference
         END
       END
       HEAT TRANSFER MODEL: 
         Homogeneous Model = True
         Option = Thermal Energy
       END
       TURBULENCE MODEL: 
         Option = Laminar
       END
     END
     FLUID PAIR: Steam | Water
       INTERPHASE TRANSFER MODEL: 
         Option = Free Surface
       END
       MASS TRANSFER: 
         Option = None
       END
       SURFACE TENSION MODEL: 
         Option = None
       END
     END

[fabfi]

Maybe the picture helps to understand the problem. Displayed is the volume fraction of water. Over time it gets much worse.

[shrirang]

Why did you give an opening boundary condition?
How about defining the lower wall as wall with the hot water temperature?

[fabfi]

Yep tried that as well. But only helped a little. In the end I had stratified water in the big volume (hot water has 98C and cold has 20C). Maybe I could define a wall heat flux depending on the average temperature in the hot volume but still it is not well distributed.

[shrirang]

Defining wall with the hot temperature should satisfy your need, as it is similar to having a fluid layer of that temperature at that position neglecting buoyancy.

[fabfi]

Originally Posted by shrirang

Why did you give an opening boundary condition?
How about defining the lower wall as wall with the hot water temperature?

--> I try to keep the temperature in the hot zone constant by having a hot backflow into the domain when cold water leaves it.

I am open for other ideas. I could also make the hot volume veeery big but i try to avoid this due to model size reasons.

[fabfi]

Originally Posted by shrirang

Defining wall with the hot temperature should satisfy your need, as it is similar to having a fluid layer of that temperature at that position neglecting buoyancy.

In the picture you can see a thin layer of hot water at the bottom and at the right wall. Still a little colder water stratifies above because it heats up too slow.

Dont be confused by the additional temperature profiles in th solids and the slightly different geometry (top right and left).

[shrirang]

You said that the hot water is a big domain physically. Is it modelled of the same scale?

If the cold water domain is very small in size, you wouldn't need any additional heat source other than initializing at high temperature.

Are the size of domain in the simulation exactly scaled from the physical one you want to compare?

[fabfi]

Nope. The warm zone is just a tiny part of the real volume. I only look at a small detail of the construction. Sure, I could make it bigger but I guess the problem would still persist.

[shrirang]

You can just have a quick hand calculation for energy balance before and after mixing and get an idea how much temperature to expect.

[fabfi]

Got a solution, at least for the next steps. I stop Mass and Momentum transfer over the interface from water to air and allow only thermal interface flux. Thus, it behaves like a wall.

Actually, I wanted to have evaporation and condensation in a later state of the model as well. So for that I need the interface flux and I will have to come back to problem. But for now, this should be fine.

Btw: I also tried it with a heat source as function of warm water average temperature. But it is not mixing up perfectly.

[JuPa]

Tips:
1) Solve the momentum and turbulence equations as homogeneous, but the energy equation as inhomogeneous.
2) For a better result switch everything (except turbulence) to inhomogeneous
3) The free surface sharpness is mesh dependent - refine the mesh where you expect the free surface to be
4) Make sure you're using the correct interfacial area density. If you get bubbly or droplet flow use the particle model. If it's all stratified use the free surface model. If its both then use the mixture model and define your own interfacial area density.
5) Couple volume fractions to the momentum and continuity equations for greater stability. This option is in solver control.
6) Use a specified blend factor of 1 as opposed to high resolution.
7) Thermal time scales are longer than molecular time scales. Freeze the flow fields and only solve the energy equation first to accelerate solution convergence.