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 = 1.0e9 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) = 2.58973e08 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 = 9.36251e05, No Iterations 119 DICPCG: Solving for pd, Initial residual = 0.000170606, Final residual = 7.79927e05, No Iterations 1 time step continuity errors : sum local = 4.05377e08, global = 4.82635e11, cumulative = 1.09681e06 DILUPBiCG: Solving for epsilon, Initial residual = 0.000297702, Final residual = 1.91179e07, No Iterations 1 DILUPBiCG: Solving for k, Initial residual = 0.000238782, Final residual = 4.38367e07, 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 = 8.73864e05, No Iterations 792 time step continuity errors : sum local = 0.000151443, global = 2.20443e07, cumulative = 1.17686e07 DILUPBiCG: Solving for epsilon, Initial residual = 0.999984, Final residual = 8.08445e06, No Iterations 27 DILUPBiCG: Solving for k, Initial residual = 0.874895, Final residual = 4.33633e08, 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 = 4.06343e06, No Iterations 33 DILUPBiCG: Solving for k, Initial residual = 0.0593825, Final residual = 1.15867e06, 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. 
Quote:
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 
All times are GMT 4. The time now is 02:00. 