[hwangpo]

Hey, guys!
I am simulating a two-layered flow in a box with an outlet and the case is 2-d simulation. (See details in the attached picture)

I used two-phase homogeneous model, with free surface option in ''Interphase Transfer''.

The inlet B.C. used 'opening', of which the opening pressure (relative pressure) is 'pressure' which is defined in EXPRESSIONS (see below).

The outlet used 'normal speed':4.27 m/s

The top surface is 'Free slip wall' and others are 'no-slip' walls.

EXPRESSIONS:
h0=72 [m]
VolumeFraction_1 = step((y-h0)/1[m])
VolumeFraction_2 = 1 - VolumeFraction_1
rho1 = 998.0[kg m^-3]
rho2 = 998.5[kg m^-3]

pressure = rho1*g*(87[m]-y)*step((y-h1)/1[m])+(rho1*g*15[m]+rho2*g*(h1-y))*step((h1-y)/1[m])

I choose the 'buoyant model', -g in y-direction.

And the results were very bad, definitely wrong.
I can not figure this out.
Your help is very appreciated.

bht_2d_2p.jpg

bht_2d_2p_004.jpg

bht_2d_2p_005.jpg

To be clear, the black line is used to explain two layers' interface which doesn't exist in the model.

[ghorrocks]

What are the two fluids? They only have a small density difference so the difference sounds like a temperature difference or maybe salinity. Either way this does not sound like a multiphase simulation - both phases are liquid, so there is only one phase. That is why it is not converging, you have not selected an appropriate physical model.

[hwangpo]

Originally Posted by ghorrocks

What are the two fluids? They only have a small density difference so the difference sounds like a temperature difference or maybe salinity. Either way this does not sound like a multiphase simulation - both phases are liquid, so there is only one phase. That is why it is not converging, you have not selected an appropriate physical model.

Thank u for your reply.
It can be modeled by using two-phase model indeed, as my friends in Canada did that successfully (sadly they graduated).
The problem I care about is can the top layer water be withdrawn through the outlet.
And you know, I was stuck.
I am wondering if things are going right by changing the simulation to unsteady?
any suggestions?
Thanks a lot.

[ghorrocks]

Multiphase models are designed to model multiple phases. This sounds obvious but it really means it is not suitable for single phase flows. If somebody else modelled it with a multiphase model then they are wrong and you should not repeat their mistake.

So what are the two fluids? Both thermal differences and salinity differences are better modelled with other approaches.

[hwangpo]

Copy that. Thank you so much.
The difference between the two water layers exactly caused by temperature like what you talked above. what do you suggest then?
I simulated this thermal stratificated tank before, using a user-defined water of which density is varying with elevation (so is the temperature) and meanwhile heat transfer was concerned. It is not that good too. The rate of convergence is very slow(about 2000 steps).
thank you very much for your help. Looking forward to your reply.

[hwangpo]

Originally Posted by ghorrocks

Both thermal differences and salinity differences are better modelled with other approaches.

Would you please explain what 'other approaches' are?
I really appreciate it. Thank you.

[ghorrocks]

If the density difference is from temperature then you have two choices:
1) Assume bousinessq buoyancy with a thermal model
2) Make the properties of wafer a function of temperature (and anything else important) and run a thermal model.

Option 1 is easier and more stable but is only accurate for a small range of temperatures. I suspect your difference is large enough that option 2 is required. Then you define an initial condition where the temperature is not constant and you automatically get your density difference. You also get things like thermal diffusion as well which is probably important.

[hwangpo]

Many thanks.
I am going simulate it in that way.
Very helpful ideas.

[ghorrocks]

Don't forget about how the pressure works in flows with a hydrostatic head.