interCondensatingEvaporatingFoam
 

Dears,


I need changing the value in constant/phaseChangingProperties but I don't know what the values mean in the tutorial. I need to simulate turbulent flow vapour-water in pipe.
Does anyone have any ideas of what these values are? :confused::confused:

Hi Claudio,
The Lee's phase change model is used in the tutorial condensatingVessel. The evaporative mass source is calculated as:

m_evap = coeffE * rho_liquid * alpha_liquid * (T - T_sat) when T>T_sat.
Here there is the model's source documentation:
https://www.openfoam.com/documentati...87_source.html

In literature you can find many info about the Lee's model, and what the constant coeffE means.
In this link, for instance, you will find a desciption of the phase change model used in a different solver, icoReactingMultiPhaseInterFoam: https://www.openfoam.com/documentati...ls_1_1Lee.html

BE CAREFUL: in this link there is the equation you can find in literature too; you'll see that the equation used in interCondensantingEvaporatingFoam lacks of a term (1 / T_sat), so the coefficients are defined differently.

Finally, the evaluation of the coefficient:
many numerical simulations use a different coefficient, which is not predictable. I'll try to make that simple: if you use a low value, your calculation will probably find convergence, but the accuracy won't be so good..This will make
the interface temperature be higher than T_sat (ideally you should find T_int=T_sat). On the other hand, if you use a very high value of the Lee's coefficient, you will have accurate results, but the calculation may fail. Usually, you should start with a coefficient equal to 0.1 and then see what happens in your simulation (I found even values in the orders of 10^7 ). Sometimes (T_interface - T_sat)= 1 K is a good result, but depends on the particular situation.
The coefficient that you have to put in phaseChangeProperties should be equal to the Lee's coefficient divided to T_sat.

Hope this is helpful.

Lorenzo

PS: which version of OpenFOAM are you using? I'm currently working on openFoam-v2006, and I'm interested in two-phase flow boiling inside a channel (I'm trying to use both interCondensatingEvaporatingFoam and icoReactingMultiPhaseInterFoam), so maybe we can discuss about that.

Hi Lorenzo. Thanks for your reply.

Your information will help me a lot.

My OpenFoam version´s v2006. My interest is in a two-phase flow cooling inside pipe.

Yes, we can discuss how to simulate our cases in interCondensatingEvaporatingFoam.

Regards.

All right, I made the example taking into account the evaporation rate, but for the condensation process it is the same thing except for the gradient of temperature, which is (T_sat -T) instead of (T - T_sat).

I tried using the "constant" phase change model in OpenFoam v1812 for annular flow boiling. The evaporation rate is distributed uniformly on the liquid zone, but I want the evaporation process to be located along the interface liquid-vapor.
For that reason, I'm studying the "interfaceHeatResistance" model, which is available only for OpenFoam v2006.

It is a little challenging because I'm not so expert on OpenFOAM and C++, and there are few documentations, tutorials and forum discussions about interCondensatingEvaporatingFoam.
Let me know if you can achieve some good results and if you have any problem.

Regards.

Yes, I agree.

This model I do not know. I'm trying to simulate water-steam two-phase flow whith k-epsilon model but my simulation is blowing up. I started with first order solvers and after a while I switched to second order solvers. But the k equation is unbounding and the message in terminal is "bounding k ...." .

Exactly, there is a little documentation and tutorials for the validation of these cases. My experience with OpenFOAM and C++ started in 2018 so I'm still learning about that.

I haven't yet good results and I have many problems :)
Regards