[idefix]

Hello,

I am using the interFoam-solver. Alpha1 is characterizing the volume fraction (alpha1= 0 means: there is only gas in the cell, alpha1=1 means: there is only liquid in the cell).
Now I´ve got the problem, that alpha1 is getting negative or greater than 1 which is not realistic.

My idea is to "correct" the alpha1 after every time step.
I need something which goes into every cell: If alpha1 is negative or nearly 0 (for example 0.1e-6), alpha1 should be put to 0. If alpha1 is greater than or nearly 1, alpha1 should be put to 1.

I would put this function in tha alphaEn.H - file after the for loop.

Can anybody help me?

Thanks a lot

[Phicau]

Hi,

I would not suggest doing this, as MULES handles itself the boundedness, continuity and conservation of alpha1. Although you may obtain vales slightly lower than 0 or larger than 1, if your BCs are correctly set, these will only be on the order of machine precision.

However, to do what you asked:

threshold = 0.01; // You name it
alpha1 = alpha1 * pos(alpha1-threshold) * neg(alpha1-1+threshold) + pos(alpha1-1+threshold)

Best,

Pablo

[sophie_l]

Hi Pablo,

I am using interFoam/waveFoam as well. I remember in the code, the value of alpha1 is restricted between 0 and 1. However, the case I am running at the moment gives out results like this, where Max(alpha1) = 1.57337. But the case is still running even though.

Courant Number mean: 0.00685244 max: 0.558313
Interface Courant Number mean: 6.62914e-05 max: 0.558313
deltaT = 0.00132421
Time = 0.186161

MULES: Solving for alpha1
Liquid phase volume fraction = 0.666668 Min(alpha1) = 0 Max(alpha1) = 1.16009
MULES: Solving for alpha1
Liquid phase volume fraction = 0.666668 Min(alpha1) = 0 Max(alpha1) = 1.57337
GAMG: Solving for p_rgh, Initial residual = 5.1474e-05, Final residual = 6.30767e-06, No Iterations 1
time step continuity errors : sum local = 1.13037e-05, global = -3.39547e-08, cumulative = -6.81206e-06
DILUPBiCG: Solving for epsilon, Initial residual = 0.00528157, Final residual = 7.39422e-09, No Iterations 7
DILUPBiCG: Solving for k, Initial residual = 0.00656354, Final residual = 3.16796e-09, No Iterations 8
ExecutionTime = 1408.43 s ClockTime = 1465 s

I am thinking it should be due to the input boundary conditions, however, I haven't got a clue where the check should start with. Do you some suggestions on this please?

Thanks a lot!
Sophie

[Phicau]

Hi

it is very likely that your alpha1 unboundedness is caused by the BCs. I suggest you take a look at this post for BC reference:

http://www.cfd-online.com/Forums/ope...ed-topics.html

if that does not solve your problems, explain your case there and I am sure they will be able to help you.

Best,

Pablo

[ngj]

Hi Sophie,

From the snap-shot of the log file, it is clear that:

1. You are not solving the momentum equation.

2. You are only solving the pressure equation one (1) time per time step.

If you relate that with the fact that interFoam/waveFoam is based on a PIMPLE-algorithm, then you will have no chance what so ever in obtaining mass conservation on the cell level; in your case the error in mass conservation is considerable. This is most probably the reason for the unboundedness of alpha1.

So: start solving for the momentum equation and have 3-4 iterations in the pressure equation per time step. This will greatly improve on your mass conservation problems and therefore improve on the boundedness of alpha1.

Kind regards,

Niels

[sophie_l]

Hi Niels,

Thank you so much for your reply. Really appreciate your help so far!

That's quite inspiring really. I'll resort to the code to work it out. By the way, I am using OF 1.7.1 based on PISO algorithm. However, in the cases I ran earlier, I didn't see alpha1 could be larger than 1.5, at most 1.0*.

Many thanks,
Sophie

[ngj]

Hi Sophie,

If you are using the PISO algorithm, the problem is at least as bad as using PIMPLE (though, if your relaxing factors are 1, then the results should be identical).

You do not need to modify/read the code, but merely change some keywords in fvSolution.

Furthermore, I can recommend that you read the section on the PISO algortihm in

@book { Ferziger2002,
Author = {Ferziger, J. H. and Peric, M},
Title = {Computational Methods for Fluid Dynamics},
Publisher = {Springer},
Year = {2002},
Edition = {3rd},
}

which will aid you in understand the importance of the settings for the PISO-algorithm.

Kind regards,

Niels

[sophie_l]

Hi Niels,

Thanks a lot!

Fortunately, I've borrowed this book from the library. I'll read this part right now.

Cheers,
Sophie

[idefix]

Hi,

the discussion is really helpful for me and I have got one question to it.

My simulations are not running very well. Soon after the beginning the velocities are increasing and as a result my time step is decreasing till the simulation stopps ( I am using adjustableRunTime). The turbulent viscosity is getting very small too.
I am using the k-epsilon-model.
At the beginning I thought that alpha1 is the reason for this behaviour but the discussion here gives some hints that the problem could be somewhere else.

Is there a possiblity to change something in the fvSolution-file so that the simulation get stable?

At the moment my fvSolution-file looks like:

solvers
{
pcorr
{
solver PCG;
preconditioner DIC;
tolerance 1e-10;
relTol 0;
}

p_rgh
{
solver PCG;
preconditioner DIC;
tolerance 1e-07;
relTol 0.05;
}

p_rghFinal
{
solver PCG;
preconditioner DIC;
tolerance 1e-07;
relTol 0;
}

"(U|k|epsilon)"
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-06;
relTol 0;
}

"(U|k|epsilon)Final"
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-08;
relTol 0;
}
}
PIMPLE
{
momentumPredictor no;
nCorrectors 3;
nNonOrthogonalCorrectors 0;
nAlphaCorr 1;
nAlphaSubCycles 4;
cAlpha 2;
}

My log-file is:

Courant Number mean: 0.001746147011 max: 0.512101182015
Interface Courant Number mean: 2.50102364228e-05 max: 0.0844578543383
deltaT = 3.4147974996e-18
Time = 0.0041231153508954621

MULES: Solving for alpha1
Phase-1 volume fraction = 0.0910985755396 Min(alpha1) = -8.28923892037e-44 Max(alpha1) = 1.00000001104
MULES: Solving for alpha1
Phase-1 volume fraction = 0.0910985743502 Min(alpha1) = -3.51986718636e-44 Max(alpha1) = 1.00000001103
MULES: Solving for alpha1
Phase-1 volume fraction = 0.091098573153 Min(alpha1) = -4.940549133e-45 Max(alpha1) = 1.00000001103
MULES: Solving for alpha1
Phase-1 volume fraction = 0.0910985719483 Min(alpha1) = -3.27296438965e-44 Max(alpha1) = 1.00000001102
DICPCG: Solving for p_rgh, Initial residual = 0.0269677660092, Final residual = 0.00113281797768, No Iterations 2
time step continuity errors : sum local = 3.66942289335e-07, global = 1.44616781464e-07, cumulative = 0.000266660876022
DICPCG: Solving for p_rgh, Initial residual = 0.00387752776814, Final residual = 0.000186226585041, No Iterations 13
time step continuity errors : sum local = 6.10538629187e-08, global = 1.86907321117e-08, cumulative = 0.000266679566754
DICPCG: Solving for p_rgh, Initial residual = 0.000664946844126, Final residual = 9.53727056345e-08, No Iterations 120
time step continuity errors : sum local = 3.12780800404e-11, global = 1.96037099123e-12, cumulative = 0.000266679568714
DILUPBiCG: Solving for epsilon, Initial residual = 0.00538752754077, Final residual = 4.08274384377e-10, No Iterations 2
DILUPBiCG: Solving for k, Initial residual = 0.00378438227684, Final residual = 2.31895835788e-09, No Iterations 1
max(k) = max(k) [0 2 -2 0 0 0 0] 2.60958163608e+13 min(k) = min(k) [0 2 -2 0 0 0 0] 0.00172278530058
max(epsilon) = max(epsilon) [0 2 -3 0 0 0 0] 2.84510295356e+22 min(epsilon) = min(epsilon) [0 2 -3 0 0 0 0] 15.772024055
max(U) = max(U) [0 1 -1 0 0 0 0] (1.3707489336e+12 2.3034155804e+12 9.11378593063e+12) min(U) = min(U) [0 1 -1 0 0 0 0] (-1.87325084502e+12 -3.151035603e+12 -5.6941716128e+12

ExecutionTime = 29474.2 s ClockTime = 29593 s

Thanks a lot

[ngj]

Hi Idefix,

Try running your simulation without a turbulence closure. Your turbulence quantities are diverged, so poor boundary conditions on k/epsilon could be the source of your crash.

Kind regards

Niels

[idefix]

Hi Niels,

thanks for your answer but I am not so familiar with OpenFoam.
How can I run my simulation without turbulence closure?
Going away from URANS?

thanks again
Idefix

[ngj]

Hi Idefix,

Open the file

constant/RASProperties

and change your current RASModel to

RASModel    laminar;

Kind regards

Niels

[idefix]

Hi Niels,

in my case I´ve got a pipe flow and the Reynolds-numbers says that I have got a turbulent flow.

For my understanding I should calculate the flow turbulent.

Is there something else I can try?

Thanks a lot,
Idefix

[ngj]

Hi Idefix,

My suggestion is only meant for debugging. Turning off the turbulence, you can lower the complexity and see, whether the turbulence model is the cause of your problems. If yes, you know that you need to change e.g. the boundary conditions to stabilise the model.

You could also try to use upwind on all of the divergence schemes in fvSchemes.

Kind regards

Niels