Hi Kimia,

Go through this tutorial.

Thank you very much for the tutorial. It was very helpful. I believe the tutorial defines a wall as the initial boundary. Can you tell me how to define a predefined shape like a hemisphere as a droplet for the initial interphase?

Hi Kimia,

Computational study of evaporation in fluent is effected by various factors -

1. Weather you are using UDF or inbuilt Lee model of fluent.

2. Setting Evaporation and Condensation frequency (Important One)

3. Patching of Volume Fraction and Temperature in the domain.

Although, I think hemispherical interface should be maintained itself depending upon the surface tension and contact angle settings in the fluent.

Moreover, specific suggestions can be provided if more info is available on the geometry and input parameters.

Thank you

Regards,

Vidit Sharma 

How about the thought that the source terms computed by the UDF are incorrect?

If Courant number is very high, it indicates source terms are erroneous which lead to poor convergence.

The mass source term is computed by

m_dot = (dm/dt) x interfacial area

where dm/dt is the evaporation mass flux (kg/m2/s) computed from Hertz-Knudsen-Schrage's (H-K-S) model, m_dot = mas source term (kg/m3/s) which is negative for liquid phase and positive for gas phase.

The trick here is to calculate interfacial area which can be written as

A_int = constant x gradient (alpha)

where the constant = f (alpha) and alpha is volume fraction.

The energy source term (J/m3) for the mixture phase is computed as

E_dot = m_dot x lambda

where lambda is the latent heat of vaporization.

The accommodation coefficient in H-K-S is the probability of vapor molecule escaping the interface and is indeed an adjustable parameter ( 0 - 1.0) which needs to be tuned to match experimental data.

Just on the other note, Geo-reconstruct method with PISO pressure-velocity coupling for the VOF method is just fine for achieving convergence.

Hope it helps,

SM

Thank you so much for your answer. Can you help me with the constant that you mentioned in the A_int? From the literature I've always thought the interfacial area that has the unit of 1/m is the gradient of volume fraction. This is what I have been using in my project. Do you know how I can get that constant? Thank you so much. 

Hi,

Did you achieve any progress, please?

The answers here helped me a lot with my simulation. I have not got the correct answer yet but many of my problems are solved using suggestions here. 

Hi, I am working on the simulation of condensation in a tube. I have also used VOF and the inbuilt Lee model. However, I am not getting any condensation. From what I've understood in the user guide, FLUENT automatically adds the source terms in energy, momentum (not for VOF). Do I need to define mass source term for each phase to observe condensation? If so, am i adding source terms to continuity eqn? Thank you

Hi. By using the embedded Lee model in FLUENT you don't need to add any sources to the equations. The model itself adds the source terms for each phase; However, if you want to monitor the rate of phase change you would need to allocate some memory for it via UDF code. 

From my experience in evaporation modeling, I couldn't be sure that evaporation is actually happening unless I would use a UDF code to compute the rate of mass transfer. 

If condensation does not happen in your case you might need to make sure that the conditions such as local temperatures are physically correct.

Hello, Thank you for your reply. I am now having condensation, but it diverges very soon. I guess the divergence is due to the condensation and evaporation frequencies, because when I put small values, it converges but with no condensation. Can anyone advice on that? Also, I observe more condensation when I put mass transfer from liquid to vapour [which seems a bit contradictory] (My primary phase being liquid). Can someone please clarify on this? Any "trivial" help/advice is most welcomed. Thank you.

If you are getting divergence you can try reducing under-relaxation factors. Or maybe try with smaller time steps. This will work if other settings are correct. Changing the mass transport from liquid to vapor is not correct.

Hello Subhasish Mitra and Kimia Montazeri,

I am also working on evaporation modeling of Hertz-Knudsen-Schrage equation by writing UDF in Fluent.

The UDF is running but not resulting in desired result to match experimental or analytical values such as Stefan Problem1.

I request to let me know where I am going wrong. My queries are:

1) Am I modeling the interfacial area density proprely? What is the constant that Subhasish was mentioning?

2) Though the simulation is running and interface is moving: This is happening only with cell size ~ 1 mm. When cell size ~ 1 micron, I could not see the interface movement. May be I have to wait for a long time with a very small time step ~1e-06?

Thanks in advance!

Hello Vidyadhar,

From a quick look at your UDF code, I can point out to a few things.

1. I don't see how your energy source terms are being applied. Are you sure you are considering the latent heat and are applying the energy source term properly at your interface? Are you applying your source to the mixture phase?

2. For calculating the interfacial area density, maybe your approach works but the expression I had used was: a=sqrt(|\nabla(\alpha)|^2). This is how I applied it in the code:

a= sqrt((C_VOF_G(c,ppt)[0])*(C_VOF_G(c,ppt)[0])+(C_VOF_G(c,ppt)[1])*(C_VOF_G(c,ppt)[1]); +(C_VOF_G(c,ppt)[2])*(C_VOF_G(c,ppt)[2]));

You can find these definitions in the papers below:

Article Microscopic analysis of thin-film evaporation on spherical p...

Article Experimental and computational investigation of vertical dow...

Article Review of computational studies on boiling and condensation

3. I am not sure what constant you are considering but generally the constant that has been used in these models is called mass accommodation coefficient. Various values are suggested for it. You should probably check out some references for it. It is usually between 0 and 1.

4. When your element size is small, limitations on Courant number will affect your time steps. For getting convergence, you usually have to use small time steps so it is reasonable that it will take a longer time for you to actually see what happens to the interface.

Thank you Kimia Montazeri for your suggestions.

1. I understood like: DEFINE_MASS_TRANSFER macro would compute the source terms in continuity, momentum and energy equations according to the mass transfer rate mentioned in the UDF and poperties(standard state enthalpy) mentioned in the properties panel.

For cross checking, I have modified my UDF to incorporate DEFINE_SOURCE macro and hooked the sources on respective mixture/phase domains. Even then, I do not see any phase change taking place.

I request you to kindly go through the modifed UDF (attached herewith) and suggest me if there is any fundamental issue.

2. I am applying sources by identifying cells where the volume fraction of secondary phase lies between 0 and 1.

Like:

if (C_VOF(cell,sec_th)>0.0 && C_VOF(cell,sec_th)

Hello,

The only way to match Stefan problems is to compute mass flux with temperature gradients at the interface. Please send me an email to [email protected]. I will be glad to help. Feel free to check my book chapter or other publications.

Best regards,

Isaac Perez-Raya

Post-doctoral Researcher

Complex Systems Simulations Laboratory

University of Wisconsin Milwaukee

Thank you Isaac Perez-Raya for replying. I have sent you an email.

Regards,

Vidyadhar K