Hi

Why don't you use the VOF model with the implicit scheme to remove the time-step limitation?

Dear Kimia Montazeri,

Selection of the time step size (dt) in a CFD simulation depends on the mesh size (dx) and the magnitude of velocities (Umax) expected to be generated in the domain. If the velocities are large, one stands the risk of out-fluxing information greater than one cell size which would make the Courant number (C) to exceed unity...this is undesirable.....hence the selection of dt should be such that C

Thank you very much for your helpful answers.I really appreciate it. I tried implicit scheme and it seems that the iterations are happening much faster and larger time steps are available. Using implicit scheme, the GEORECONSTRUCT scheme is not available in VOF model. I tried MODIFIED HRIC which seemed to work but I don't know if it is correct to use it. 

My other concern is that as the time step increases, the evaporating meniscus inside the pore starts to become distorted (in small time steps it is completely smooth). I am not sure if it is important, but since I am trying to analyze thin film evaporation, I want to make sure that it is not effecting the accuracy of the model. 

Thank you again for your help. 

Dear Kimia Montazeri,

Whilst using Modified-HRIC, it is probable that the interface between the two phases might diffuse (increase in thickness)...I had observed this with waves in FLUENT. Hence, I would advise you to observe the evolution of the interfacial region (transition region from f=0.0 to f=1.0) carefully during your simulations.

Best regards.

Shaswat

 Hello, Kimia,

       Before answering your question, I think it is better for me to inform you that your simulation is probably not suitable for micro scale using the software Fluent. Actually, in my identification, VOF is a method using in engineering prediction to determine the interface development between two different phases. However, due to its limitation in contorlling equations, it is weak in physical researches and identification, otherwise you have a set of  experimental data as benchmark.  The solution of each phase is independent, whereas the interaction only decides at the interface. Detailed equations can be seen in Fluent help files and I suggest you carefully read it.

      If you just wish a consequence from Fluent,  you might use Morteza's advice using  the implicit scheme  to neglect the time-step limitation. But this will make the result not in a accurate assumption with in CFD identification.  In Shasawat's advices,  he present a clear explanation of  accurate selection of the time step size (dt) in a CFD simulation, which depends on the mesh size (dx) and the magnitude of velocities (Umax) expected to be generated in the domain. This is also the meaning of  the Courant number (C).

     Finally, I think the process you simulated  under a micro scale is an unsteady process, thus , it should not reach to a  convergence step. I feel what you need is an evaporation process other than an evaporation result, isn't it?  Therefore, If you care about the initial development, only if  the right delta time should be present. If you are just care about the final evolution state, you can use a large time step at the beginning and switch it the smaller time-step to make sure whether the consequence  is a expected result.

     Hope these suggestions may help you. 

Dear Kimia,

First of all you should make clear about what is the meaning of "it impossible to reach convergence". What I understand from this statement is that you are trying make the point that it takes huge amount of time for the simulation of your problem. Typically, these class of problems (phase change) takes longer physical time as it requires small time steps. Therefore, the time step you are using seems to be correct. 

There are following criteria for time steps in two-phase flows:

1. CFL (Already people have mentioned. In fact, Shashwat has discussed in detail.)

2. Time step from diffusion. 

3. Time step from surface tension.

If your time step size is smaller than each of the above criteria then you should not have any trouble. 

Now if flow is dominant by advection then CFL time step restriction applies. Probably in your case CFL has least importance in my opinion.

Check for other two. One of them should work. Therefore, you are bound to work with small time steps.

Best

Zinjala Hiteshkumar

Hello Kimia,

It seems that you are trying to simulate a micro-scale problem via macro-scale tools ( VOF), so maybe it will be helpful to think about some alternative solution strategies which contain more compatibility between the problem and the simulated model.

Also you may use open source micro-scale codes in such areas that I will be happy to introduce you some ,if you are interested in.

wish success in your reasearches,

Sh.Ghorbanifar

Correction:

Researches

In my opinion you must go with VOF HRIC model to carry out your simulation

Thank you all for the great suggestions. I really appreciate your help. I could manage to reduce the time step to the order of 1e-07 s with the explicit scheming. Seemed like I had an error in my source terms in the UDF that caused many errors and affected time steps as well. However, I get some temperature sinks in near the interface areas (Temperature limited to 1K or some very low temperatures). I know it might be because of the high heat source but I cannot figure out what to do about it. I appreciate any suggestions. Thank you very much.