[thr]

Hello,

im try to simulate sloshing in a closed tank.

I use OF11 and based on the tutorial sloshingTank6DoF i built up my own simulation. In the end i want the forces acting on the tank due to the liquid sloshing. When i read the data from the postProcessing folder i get really confusing Oscillations. I have no clue why this is happening. I have tried several different options in fvSchemes and fvSolution.

controlDict:
application foamRun;

solver incompressibleVoF;

startFrom latestTime;

startTime 0;

stopAt endTime;

endTime 1;

deltaT 0.0001;

writeControl adjustableRunTime;

writeInterval 0.1;

purgeWrite 0;

writeFormat binary;

writePrecision 9;

writeCompression off;

timeFormat general;

timePrecision 9;

runTimeModifiable yes;

adjustTimeStep yes;

maxCo 0.4;
maxAlphaCo 0.4;

maxDeltaT 0.01;

functions
{

forces
{
type forces;
libs ("libforces.so");
patches ("sloshingCylinder");
log on;
writeControl adjustableRunTime;
writeInterval 0.001;
rhoInf 1000;
rho rhoInf;
CofR (0.4 -0.4 0.1); // Point for calculation of moments


}
}

fvSolution

solvers
{
alpha.water
{
nAlphaCorr 1;
nAlphaSubCycles 3;
}

"pcorr.*"
{
solver PCG;
preconditioner
{
preconditioner GAMG;
tolerance 1e-05;
relTol 0;
smoother DICGaussSeidel;
cacheAgglomeration no;
}

tolerance 1e-05;
relTol 0;
maxIter 100;
}

p_rgh
{
solver GAMG;
tolerance 1e-08;
relTol 0.01;
smoother DIC;
}

p_rghFinal
{
solver PCG;
preconditioner
{
preconditioner GAMG;
tolerance 2e-09;
relTol 0;
nVcycles 2;
smoother DICGaussSeidel;
nPreSweeps 2;
}

tolerance 2e-09;
relTol 0;
maxIter 20;
}

"(U|k|epsilon|omega).*"
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-06;
relTol 0;
nSweeps 1;
}
}

PIMPLE
{
momentumPredictor no;
nCorrectors 5;
nNonOrthogonalCorrectors 1;
correctPhi no;

pRefPoint (0.4 -0.4 0.1);
pRefValue 1e5;
}

relaxationFactors
{
equations
{
".*" 1;
}
}

dynamicMeshDict

mover
{
type motionSolver;

libs ("libfvMeshMovers.so" "libfvMotionSolvers.so");

motionSolver solidBody;

select all;

solidBodyMotionFunction sixDoFMotion;

CofG (0.4 -0.4 0.1);

translationRotation table;
//interpolationScheme spline;
file "$FOAM_CASE/constant/6DoF.dat";

}

6DoF.dat is a table with a frequency of 800hz. simple acceleration in x direction with 9.81m/s^2.

I have attached a plot of the force. Its the same for Fx,Fy,Fz. Every 10nth data point drops. The sloshing in Paraview look good. I think this could be a problem with the dynamictMeshDict, the forcesFunction or the adjustableTimeStep.

Best,

T

[GaspA]

Hello,


I Have the same behaviour.
I think this comes from the interpolationScheme (dynamicMEshDict) for points in 6DoF.dat. But i don't understand where exactly.


Do have somebody an idea ?



Thanks.

[thr]

Hello,

I solved this Problem. I think it is not possible to build a simulation with 6DoF.dat and ready out correct forces/moments. The only way i got good results was by giving direct accelerations to openfoam. I calculated accelerations from the given positions and used these as Input for openfoam. I really tried everything to use Position as input the same way you can see in the tutorials. Everytime you give a new datapoint(Position) you will get an Oscillation in your forces. Try using accelerations as an Input for your movement! Sorry for my late reply.

Best,

T

[GaspA]

Hello,
Thank you for your answer.
I come to the same conclusion. Which is relatively regrettable I find...
I manage to get good results with the acceleration method. However I cannot read a file containing the acceleration. Reading a table in the dictionary works correctly but I do not know the syntax to read a file. I created a post in this sense Read table to fvOptions or fvModels

Maybe you have a solution.

Thank you

Best regards


GaspA