I suggest you try to use Fluent's default under- relaxation factors for calculation. If you calculate with a lower（0.1） under- relaxation factors, the time will increase. You can try to increase the under- relaxation factors when the calculation is stable.

Following

thanks YuJiang for your answer, I've tried default under_relaxation too but it didn't work.

Hello Mahtab Alipour.

I agree with Yu Jiang

Multiphasic flows are highly innestable. First of all it would be nice if you can share the following information:

How many elements does your mesh have and of what type (hexahedral, tetrahedral, polyhedral)?

Are you simulating it as stationary or transient state?

What is your step size and how long do you want to simulate?

In general, I give you some recommendations that may help you, assuming that your simulation is in a Transitory state:

-Initially try an Implicit scheme with Body forces enabled. It can allow you to use a longer time step.

-Check that gravitational acceleration is enabled and in the right direction.

-For open channels use the VOF method with the Open Channel submodel. It is very important that you enable "Implicit Body Force" to take into account the effect of body forces.

-The fluent manuals recommend that the secondary phase be the densest. In an open canal it is usually water.

-The BC are OK, but in BC outlet I suggest you enable "Open Channel" (see Multiphase option) with "Pressure Specification Method=From Neighboring Cell" and Bottom Level (m) (check Fluent's Manuals).

-Verify that Operational Conditions is enabled.

-Turbulence model is ok.

-Use the PISO scheme for pressure-velocity coupling.

-Spatial discretization = Least Square Cell Based.

-Pressure = PRESTO!

-I suggest to use Second order discretization schemes.

-Discretization scheme for Volume Fraction = HRIC modified (less numerical diffusion than Compressive).

-Transient formulation = Bounded Second Order Implicit.

-Relaxation factors: Pressure = 0.3, Density = 1, Body Force = 0.7, Momentum = 0.3 to 0.7 (it is very critical), Volume Fraction = 0.5, k = 0.75, e = 0.75, Turbulent Viscosity = 0.75

-Check that you have a correct initialization of the problem (you can estimate initial depth water with uniform flow).

-Use a small time step (For example 0.005 s). If it shows good convergence you can increase it.

-Uses convergence monitors such as Mass Flow Rate and shear stress (Thao = pho * g * S * Rh).

-Other options: you can explore Non-Iterative Time Advancement (NITA) scheme. People think that is useful en Multiphasic Flows. I have doubt in calculations of residuales with this method, but you can explore this option.

Regards!

Hi Leonardo Henao

thanks for your recommendations those were really useful.

544418 elements are in my mesh(pave(Qurid)) and time step size is 0.01.

for No. of time steps l've used following formula

N=T/Delta t

T=Length of domain/velocity

but I changed it because it was 635000, actually I don't know how long I should simulate. can you please give me a clue about how long usually it is taken?

It was stationary but I've changed it to transient and it worked now residuals are decreasing, but I have new problem, the velocity that Fluent have calculated is far away from experimental quantity. I've considered all your recommendations but Fluent doesn't calculate satisfactory quantities for velocity.

Dear Mahtab Alipour

Regarding the mesh: where possible a hexahedral mesh is preferable, mainly in the domain of the flow of interest (in the core of the flow, so to speak, and at the water-air interface). If a completely hexahedral mesh is not possible, then it can be supplemented with a polyhedral mesh. I don't have much experience with pave mesh, but I recommend you check the following link:

https://journals.sagepub.com/doi/pdf/10.1260/1757-482X.3.1.13

Now, the number of elements seems adequate, although it may require a high computational cost as well (several hours of calculation), to simulate a few seconds. IN TRANSITORY STATE, I recommend you perform a good initialization and simulate a total time T = 5 seconds, with a time step dt = 0.005 s. Again don't discount the NITA scheme (I'm not an expert on the subject, but they say it's good for computational cost savings). I HAVE NOT MENTIONED ANYTHING ABOUT EXPLICIT SCHEMES AND THE COURANT NUMBER (I think that initially is better studing problem with implicit scheme without Courant number).

Regarding velocity I imagine you have measurements in certain zones or points. To compare it with the quantities thrown by Fluent you would have to estimate in those same zones, using points, lines or planes for example. Weighted volumes can also be used. I recommend you consult the following links:

https://www.youtube.com/watch?v=Chv4QhOLO-g

https://www.youtube.com/watch?v=dvn4I6hTZ6c

In addition to the above and before you continue with your progress, I suggest you do the following:

1). Verify that your mesh is ideal one for the problem. You will have to do a study of mesh independence (at least three different sizes). Note that air-water free surface tracking is very critical in multiphasic flow problems. If you have a very coarse mesh in this area, your result may not be correct.

2). Verify that the turbulence model you are using is suitable for the size of the cell closest to the wall. I mentioned to you initially that the turbulence model was adequate, because I'm assuming you know the implications of its use, especially near the wall. If you don't have much time to study the subject, I recommend using the k-e RNG with the Standard Wall Function, guaranteeing that 30

Dear Mahtab Alipour

It fundamentally depends on the method you are using to calculate the Navier-Stokes equation in your simulation. In fact, there are two algorithms for dealing with this issue that is SIMPLE and PISO. SIMPLE normally is being used for steady-state flow since it does not consider the term du/dt in the left-hand side of the equation, in contrary PISO is being employed for transient simulation, for it included the du/dt term. So in SIMPLE what is the hinder of divergence in the off-diagonal matrix of momentum equation term is the under-relaxation factor that is designed for the stabilization of pressure, in this regard if you wish to set your simulation up steady-state, you have to apply under-relaxation factor. The smaller the under-relaxation factor is, the more stable will be the result. On the other hand, in the case of transient simulation, you should decrease your time step, because in du/dt term smaller dt will result in bigger weight to du which makes the matrix diagonally dominant (ap matrix). That is how you can improve your convergence and it is very simple in Fluent, though you should follow the right track.

Regards,