
[Sponsors] 
March 16, 2009, 04:49 
Water flow in closed volume  rasInterFoam

#1 
New Member
Chris
Join Date: Mar 2009
Location: Europe
Posts: 19
Rep Power: 9 
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 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. 

March 16, 2009, 08:30 

#2 
Senior Member
stephane sanchi
Join Date: Mar 2009
Posts: 306
Rep Power: 10 
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. 

March 17, 2009, 04:31 

#3 
New Member
Chris
Join Date: Mar 2009
Location: Europe
Posts: 19
Rep Power: 9 
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! 

March 17, 2009, 08:42 

#4 
Senior Member
Matvey Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 330
Rep Power: 11 
Maybe you should try playing with laplacian and interpolation schemes  try moving from linear to upwind or limitedLinear


March 17, 2009, 10:15 

#5 
New Member
Gareth
Join Date: Mar 2009
Posts: 24
Rep Power: 9 
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. 

March 17, 2009, 11:01 

#6  
New Member
Chris
Join Date: Mar 2009
Location: Europe
Posts: 19
Rep Power: 9 
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. 

March 18, 2009, 11:46 

#7 
New Member
Chris
Join Date: Mar 2009
Location: Europe
Posts: 19
Rep Power: 9 
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) 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. 

March 20, 2009, 04:11 

#8 
New Member
Chris
Join Date: Mar 2009
Location: Europe
Posts: 19
Rep Power: 9 
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 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
RasInterFoam cavitation  maritozzo  OpenFOAM Running, Solving & CFD  2  December 6, 2005 15:09 
Flow in a Closed Loop  John Collins  Main CFD Forum  2  February 27, 2003 11:26 
Time dependant discharge from a closed volume  Chris Rand  FLUENT  2  November 8, 2002 08:44 
closed casing with fan and water  Tom  Main CFD Forum  0  August 27, 1999 01:16 
Pulsatile blood flow in closed loops  Michael F. Wolf  Main CFD Forum  3  July 1, 1999 16:37 