Water flow in closed volume - rasInterFoam
 

Hallo everybody,

So far I got very good experience with OpenFOAM multiphase solvers, but now I met some problems and I hope that will find some help here.

I am using 1.5 version rasInterFoam solver.

My domain consists of volume as shown below with one inlet and two outlets. Rest are walls.

My boundary conditions are:
- inlet – water :
u = 2m/s, pd = zeroGradient, gamma =1
- inside of the domain I got air.
- outlet :
u = zeroGradient, pd = 0

http://img4.imageshack.us/img4/3420/99835949.th.png

http://img25.imageshack.us/img25/6259/17950717.th.png

Turbulence model – kEpsilon.

My problem is that from the very beginning Courant number is increasing for the fixed Dt . I have started with Dt = 0.00002 and Co was oscillating about value 0.15. After short time Co started to grow and simulation crashed at t = 0.23 s with Co = 5.63934e+16

I have also run simulations for the smaller values of Dt, even up to value Dt = 1.0e-9 but always with the same results. In each case simulation crashes at certain simulation time t = 0.23.

Here you can see example part of the log file, at the time t=0.18 s:

Courant Number mean: 0.00256311 max: 0.174324
Time = 0.18096

MULES: Solving for gamma
Liquid phase volume fraction = 0.0223764 Min(gamma) = -2.58973e-08 Max(gamma) = 1
DICPCG: Solving for pd, Initial residual = 0.00615942, Final residual = 0.000386212, No Iterations 2
DICPCG: Solving for pd, Initial residual = 0.000678794, Final residual = 9.36251e-05, No Iterations 119
DICPCG: Solving for pd, Initial residual = 0.000170606, Final residual = 7.79927e-05, No Iterations 1
time step continuity errors : sum local = 4.05377e-08, global = 4.82635e-11, cumulative = -1.09681e-06
DILUPBiCG: Solving for epsilon, Initial residual = 0.000297702, Final residual = 1.91179e-07, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 0.000238782, Final residual = 4.38367e-07, No Iterations 1
ExecutionTime = 538.81 s ClockTime = 540 s

and shortly before it has crashed:

Courant Number mean: 0.0192395 max: 45.0056
Time = 0.23218

MULES: Solving for gamma
Liquid phase volume fraction = 0.049607 Min(gamma) = -326.245 Max(gamma) = 504.761
DICPCG: Solving for pd, Initial residual = 0.619894, Final residual = 0.0581804, No Iterations 112
DICPCG: Solving for pd, Initial residual = 0.928535, Final residual = 0.091204, No Iterations 149
DICPCG: Solving for pd, Initial residual = 0.96074, Final residual = 8.73864e-05, No Iterations 792
time step continuity errors : sum local = 0.000151443, global = 2.20443e-07, cumulative = 1.17686e-07
DILUPBiCG: Solving for epsilon, Initial residual = 0.999984, Final residual = 8.08445e-06, No Iterations 27
DILUPBiCG: Solving for k, Initial residual = 0.874895, Final residual = 4.33633e-08, No Iterations 2
ExecutionTime = 5605.74 s ClockTime = 5629 s

Courant Number mean: 7.52882 max: 280479
Time = 0.2322

MULES: Solving for gamma
Liquid phase volume fraction = 0.0489311 Min(gamma) = -1.13696e+07 Max(gamma) = 7.90837e+06
DICPCG: Solving for pd, Initial residual = 0.979423, Final residual = 658.541, No Iterations 1001
DICPCG: Solving for pd, Initial residual = 0.996411, Final residual = 3.04765, No Iterations 1001
DICPCG: Solving for pd, Initial residual = 0.998729, Final residual = 10.466, No Iterations 1001
time step continuity errors : sum local = 1.13257e+12, global = 5.43929e+06, cumulative = 5.43929e+06
DILUPBiCG: Solving for epsilon, Initial residual = 0.999699, Final residual = 4.06343e-06, No Iterations 33
DILUPBiCG: Solving for k, Initial residual = 0.0593825, Final residual = 1.15867e-06, No Iterations 16
bounding k, min: -0.00225506 max: 3.37869e+12 average: 3.88599e+08
ExecutionTime = 5627.47 s ClockTime = 5651 s

My mesh consists of 332700 hexahedra elements. checkMesh doesn't plot any errors.

I can't figure out what's the reason of this behave. My first thought was to check values of the velocities when simulation crashes. But for the last written results I don't see any unphysical values. I don't know what else might influence Co number.

So, dear forumers do you have any idea what might be wrong. I would appreciate any help, any hint.

Hi Chris,

I have the same problem using rasInterFoam for ship hydrodynamics.

I have tried both solutions :
1. To have a fixed small dt. But suddemtly Co increases a lot and the computation crashes.
2. To leave the dt free to change with a fixed maximum Co value. After a while Co increase ans so dt decreases to much (until 10^-8) ... and the computation crashes.

I have modified the parameters of the fvSolution and FvSchemes files but without success.

I think that the main problem is the initialization for transient runs !

Any help would be usefull !

Stephane.

So I am not the only one who struggle with rasInterFoam.

Problem is that so far I had very good impression with OF multiphase capabilities and would like it to stay like this:)
And I would realy appreciate if someone familiar with this could say something.

I hope it's just a matter of settings or some wrong assumptions.

Thanks in advance!

Maybe you should try playing with laplacian and interpolation schemes - try moving from linear to upwind or limitedLinear

I've also got a problem with rasInterFoam, in an open channel situation. Again, delta t goes very small, and the courant number explodes, crashing the simulation.

I am a bit of a beginner so haven't been able to figure out a fix yet unfortunately.

Hi Matvej,
I have already played with these, no success.
I think that changing discretisation scheme during the simulation shouldn't influence convergence so much - considering case which was running well at the beginning.
But of course I am not an expert and might be wrong.

Hi everybody,

in order to sort my problem I have performed some other test cases. I created new geometry (simple cuboid) with dimensions similar to my initial case and with perfectly orthogonal mesh. Inlet and outlet I have placed in the same areas.
Initial conditions (apart from velocity, now it's 1m/s) were the same.

Now simulation runs without any problems and converges within each timestep.

Below you can see some screenshots:
(free surface is coloured with velocity)

http://img6.imageshack.us/img6/6972/00004.th.png

http://img7.imageshack.us/img7/1554/00028.th.png

http://img6.imageshack.us/img6/9555/00070.th.png


Now I am a bit confused. I am happy because solver works well but on the other hand I would never expect that rasInterFoam is such mesh sensitive.

Good morning,

I have managed to solve my problem. It was necessary to upgrade a bit boundary conditions.

At the outlet I used new boundaries as follow:

pd

outlet
{
type totalPressure;
U U;
phi phi;
rho none;
psi none;
gamma 1;
p0 uniform 0;
value uniform 0;
}


U

outlet
{
type pressureInletOutletVelocity;
phi phi;
value uniform (0 0 0);
}


Now simulation runs well. Converges within each time step and I don't observe any unexpected behave.

However I got the feeling that liquid doesn't leave my domain as quick as I would expect.

I am not pretty sure if my assumptions at the outlet are correct so I would really appreciate if someone could veryfy this.

Have a nice day!
chris