Liquid Water Free Surface Evaporation
 

I am trying to implement interfacial component transfer between liquid water and air.

I have a 50m high cylinder with a radius of 15m, where the bottom and side walls are modelled as no slip walls. The top is modelled as an opening with a 0atm relative pressure and a temperature of 298K.
I have succesfully been able to create two homogeneous phases with a clear free surface at the interface by simply creating two fluid types in the domain.

Buoyancy and thermal heat transfer is included, but I further wish to couple the two phases to allow water to evaporate into the air after placing an point energy souce by the surface. How can I go about coupling the phases?
Thanks

What does the free surface do? Is it always flat or close to it? Does it go up and down? Or does it have waves, splashing and/or foam?

Each of these different states should be modelled differently.

For now I just have it as a stationary free surface. Am I right in thinking that I will have to create 3 materials. The liquid water, Air- water vapour mixture and water liquid-vapour mixture?

I tried to go about this way, but I couldn't seem to find the option for component interfacial transfer. I wish to model it through Raoult's law.

For now I just have it as a stationary free surface. Am I right in thinking that I will have to create 3 materials. The liquid water, Air- water vapour mixture and water liquid-vapour mixture?

I tried to go about this way, but I couldn't seem to find the option for component interfacial transfer. I wish to model it through Raoult's law.

Thanks very much for replying

If the interface is stationary then I would consider having them as separate domains and not use a multiphase model at all. Then you can impose the free surface transfer functions as interface conditions.

Even if the interface moves up and down you can do this with moving mesh.

But if waves, churning, foaming or bubbles are important this approach will not work.

Hi all,

I am currently trying to simulate something extremely similar to njw's case. It is an evaporation from water in a open cylinder heated from the sides. The temperature of the bulk fluid does not exceed boiling point(saturated temperature), so there is only heat transfer by convection in the cylinder, with evaporation at the top open end of the pipe.

However, one difference from njw's case is that the free water surface will be gradually moving downwards as water evaporates from the cylinder. The cylinder is thin, around 5mmx0.5m. Hence, mass loss by evaporation will have a significant impact on the water level.

Does any one have any advice on how I can model the evaporation at the top surface?

Thank you so much in advance.

Why are you modelling this with CFD? Why can't you just model this with simple control volume approaches?

Hi Sir, thank you for you reply. Sorry but could you explain how I can go about solving this by control volume method? Or do you have any references that you would recommend? The heat transfer texts I can find at does not seem to have a method for solving this problem.

Thank you in advance!

I've done a simulation like this with success. The steady state solution is an empty tank. So you must be interested in the transient. What are you hoping to achieve from the simulation?

Treat the liquid domain as a control volume, with a specified volume and temperature. Work out the temperature change, the evaporation (mass loss) and volume change for that time step, and iterate over time. Simple(ish), and no CFD required.

Hi
My project is modeling of surface evaporation in dams, Can i model the evaporation by using CFD? Many people told me you can not do this. can you help me about this problem?

Thank you so much .

You can model evaporation in CFX. But the question is more: If you are modelling evaporation in a dam do you need a CFD solver to do it?

Why do you want to model evaporation in a dam? What will you learn other than that the water slowly moves from the dam into the air and the water level slowly goes down?

my aim is to show that water storage behind dams evaporate more quickly than when water flowing on the ground .

What physical process makes dams evaporate faster?

when the thickness of (height of ) water is too high

How does the water height increase the evaporation rate?

Evaporation from a free-surface
 

Hi everyone,

I do have the same problem (evaporation from a free-surface) which I would like to solve with CFX. This is a simple problem of a 2D domain with the domain occupied by water and air (water and air are separated with a clear interface). The water and air never mix, so the homogeneous free-surface model is enough. The interface will move due to evaporation (and mass conservation).

Please note I'm interested in CFD modeling of this problem not analytic solutions. I highly appreciate if anyone can let me know if they have ever solved this with CFX or are aware of any paper/article/video/tutorial that explains how to solve this with CFX.

Thanks :-)

I have never done this type of model. CFX should have the necessary models to do it. But do not be confused into thinking this is a simple simulation - multiphase with phase change mass transfer is never going to be straight forward.

Your best bet to get an example to start you off is to contact ANSYS support.

Thanks for the reply.

I have to agree with you. This problem, although incredibly easy looking, is actually quite complex. And we also have problems with spurious currents around the interface. And in agreement with you, I think mass-transfer in multiphase flows is still on its R&D phase and is not quite robust yet.

Spurious currents at the interface is a common problem with free surface models with surface tension. So only turn the surface tension model on if you really need it.

I strongly disagree that mass transfer in multiphase flows is R&D only. There are many industries which use is successfully and accurately. But it needs a skillful, experienced CFD person to drive it and requires careful derivation and validation. You cannot simply press a button and mass transfer "just works".

This is quite wrong - you will need to use the inhomogeneous approach:
- Inhomogeneous momentum to allow the phases to separate during evaporation.
- Inhomogeneous energy for both phases to allow each phase to have its own temperature fields in order to correctly model evaporation
- You can get away with homogeneous turbulence

The particle and free surface models aren't sufficient in their formulation for the interfacial area density to model evaporation from the free surface. This means you'll need to go the mixture model route. What does this mean:
1. You need to specify the interfacial length scale (I should have a paper out soon documenting how to get the appropriate length scale for the mixture model in evaporation problems)
2. You need to specify the interfacial drag. The default is 0.44 - however this is for droplets and not a free surface.

And lastly, because you'll be using the mixture model you'll need to have two continuous phases (or in your case three!). Water, and water vapour and air above the free surface.

Essentially you're solving 3 sets of momentum equations (one set for each material), 2 sets of energy equations (assume the vapour is at Tsat and you don't need to solve the energy equation for vapour), the continuity and volume fraction equations, and your turbulence equations.

Basically, what you're after isn't easy.

Ricochet,

This is an interesting view. I understood all your points except the one that you said "Inhomogeneous momentum to allow the phases to separate during evaporation.". Can you please elaborate? Basically, I have water and vapor (lets's just say we have only two phases) which are separated by an interface (I use this as an initial condition). Then, I run the case, and ideally, the interface should move due to the conservation of mass.

btw, I did run some simulation with homogeneous approach and captured the interface movement (I am still working on it to make sure it is accurate).

Thanks

There is a sudden change of phase from water to vapour at the free surface. Well, it turns out the homogeneous momentum approach cannot model this correctly. If you do this homogeneously, significant mass of water gets "carried away" above the free surface. This is a physically unrealistic result since water is more dense than vapour and should just "fall back down".

You need an inhomogeneous approach to momentum to allow the two phases to "slip" past each other. You control the amount of slip via the drag coefficient.

Hint: look at the density ratio of water to vapour at your operating pressure. It's in the order of 1000s. Do you expect a homogeneous momentum approach will successfully model a sudden change in density from 998 kg/m^3 to 0.1 kg/m^3?

This sounds extremely interesting. Could you please tell me when the paper is available? (or provide me with a title in order to set up a scholar alarm on it)

Thanks in advance :)

related to fluent
 

Can you please clarify, what mean inhomogeneous approach related to Fluent case setup. I model evaporation from free water surface in usual room conditions and need any information, how to do it.