 |
 |
 |
|
|
|
[Sponsors] | ||||
Spikes in Time-Plot of transient Sloshing Solution |
 |
|
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
January 23, 2023, 04:32
|
Spikes in Time-Plot of transient Sloshing Solution
|
#1 |
|
New Member
Join Date: Jul 2013
Posts: 21
Rep Power: 13  |
Hi everyone,
I am simulating water sloshing in a tank. An experiment has been conducted - the results can be found in various publications such as https://doi.org/10.1016/j.compfluid.2007.11.007 or https://link.springer.com/article/10...804-012-1137-y. Also, others have simulated the case using different software yielding good results. For those that do not have access to the files, here a short explanation of the case: - water sloshing in a 2D rectangular tank - tank dimensions are height = 0.6m, width = 1.2m - the tank is excited by an oscillating motion in direction of tank width - movement is sinusoidal; amplitude is 0.015m, omega is 4.4752 rad/s - pressure is recorded at multiple points in the tank - fill height is 0.36 m Before I post my case setup files etc, here a short explanation of how I am trying to simulate the case for now: - laminar case (I want to go turbulent in the long run but laminar needs to run nicely first) - interFoam for a multiphase VOF (air, water) simulation - domain movement by means of solid body motion function oscillatingLinearMotion - ddt Scheme is Euler - grad Scheme is Gauss linear - div Schemes: please take a look at file excerpt below - initialized velocity in x-direction according to movement - adjustable time step to keep Co ~ 0.5 Here are excerpts from the files I perceive to be relevant; if you miss anything please tell me and I will post it controlDict: Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2112 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application interFoam;
startFrom startTime;
startTime 0;
stopAt endTime;
endTime 50;
deltaT 0.002;
writeControl adjustableRunTime;
writeInterval 2;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
adjustTimeStep yes;
maxCo 0.5;
maxAlphaCo 0.5;
maxDeltaT 0.01;
functions{
probes
{
type probes;
libs ("libsampling.so");
// Name of the directory for probe data
name probes;
writeControl timeStep;
// Fields to be probed
fields (p);
// Optional: interpolation scheme to use (default is cell)
interpolationScheme cell;
fixedLocations false;
probeLocations
(
(1.2 0.0 0.3)
(1.2 0.0 0.426)
(1.142 0.0 0.6)
);
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2112 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default Euler;
}
gradSchemes
{
default Gauss linear;
}
divSchemes
{
default none;
div(rhoPhi,U) Gauss vanLeer;
div(phi,alpha) Gauss vanLeer;
div(phirb,alpha) Gauss interfaceCompression;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2112 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
"alpha.water.*"
{
nAlphaCorr 1;
nAlphaSubCycles 1;
cAlpha 1.5;
alphaOuterCorrectors yes;
MULESCorr yes;
nLimiterIter 3;
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-8;
relTol 0;
}
"pcorr.*"
{
solver PCG;
preconditioner DIC;
tolerance 1e-5;
relTol 0;
}
p_rgh
{
solver PCG;
preconditioner DIC;
tolerance 1e-08;
relTol 0.01;
}
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).*"
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-06;
relTol 0;
minIter 1;
}
}
PIMPLE
{
momentumPredictor yes;
nCorrectors 3;
nOuterCorrectors 100;
//nNonOrthogonalCorrectors 0;
pRefPoint (0 0 0.6);
pRefValue 0;
outerCorrectorResidualControl
{
U
{
tolerance 1e-4;
relTol 0;
}
p
{
tolerance 1e-4;
relTol 0;
}
p_rgh
{
tolerance 1e-4;
relTol 0;
}
}
}
relaxationFactors
{
fields
{
p 0.3;
pFinal 1;
}
equations
{
"U" 0.3;
"(U)Final" 1;
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2112 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
side1
{
type fixedFluxPressure;
}
side2
{
type fixedFluxPressure;
}
bottom
{
type fixedFluxPressure;
}
top
{
type fixedFluxPressure;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2112 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0.067128 0 0);
boundaryField
{
side1
{
type movingWallVelocity;
value uniform (0.067128 0 0);
}
side2
{
type movingWallVelocity;
value uniform (0.067128 0 0);
}
bottom
{
type movingWallVelocity;
value uniform (0.067128 0 0);
}
top
{
type movingWallVelocity;
value uniform (0.067128 0 0);
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2112 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
side1
{
type zeroGradient;
}
side2
{
type zeroGradient;
}
bottom
{
type zeroGradient;
}
top
{
type zeroGradient;
}
frontAndBack
{
type empty;
}
}
// ************************************************************************* //
Code:
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration | Website: https://openfoam.org
\\ / A nd | Version: 10
\\/ M anipulation |
\*---------------------------------------------------------------------------*/
Build : 10-e450dce21ea5
Exec : checkMesh
Date : Jan 23 2023
Time : 08:34:52
Host : CLEARED
PID : 928
I/O : uncollated
Case : CLEARED
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create polyMesh for time = 0
Time = 0s
Mesh stats
points: 31506
internal points: 0
faces: 62216
internal faces: 30712
cells: 15488
faces per cell: 6
boundary patches: 5
point zones: 0
face zones: 0
cell zones: 0
Overall number of cells of each type:
hexahedra: 15488
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0
Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).
Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
side1 88 178 ok (non-closed singly connected)
side2 88 178 ok (non-closed singly connected)
bottom 176 354 ok (non-closed singly connected)
top 176 354 ok (non-closed singly connected)
frontAndBack 30976 31506 ok (non-closed singly connected)
Checking geometry...
Overall domain bounding box (0 -0.1 0) (1.2 0.1 0.6)
Mesh has 2 geometric (non-empty/wedge) directions (1 0 1)
Mesh has 2 solution (non-empty) directions (1 0 1)
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (-2.26879e-17 1.88098e-14 -2.12423e-16) OK.
Max cell openness = 1.465e-16 OK.
Max aspect ratio = 1.03019 OK.
Minimum face area = 4.62542e-05. Maximum face area = 0.0014. Face area magnitudes OK.
Min volume = 9.25085e-06. Max volume = 9.8e-06. Total volume = 0.144. Cell volumes OK.
Mesh non-orthogonality Max: 0 average: 0
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 1.30476e-13 OK.
Coupled point location match (average 0) OK.
Mesh OK.
End
 Also, residual plots of the end of the simulation (last 1000 lines of the output file) are given in the attachement. For further clarity, here are the last couple of iterations from the output file: Code:
Courant Number mean: 0.0873681 max: 0.491744
Interface Courant Number mean: 0.00141919 max: 0.436737
deltaT = 0.000721168
Time = 50s
PIMPLE: Iteration 1
DICPCG: Solving for pcorr, Initial residual = 1, Final residual = 9.54101e-06, No Iterations 286
time step continuity errors : sum local = 1.63964e-12, global = 1.22774e-16, cumulative = 4.33396e-13
smoothSolver: Solving for alpha.water, Initial residual = 0.000465417, Final residual = 1.55265e-09, No Iterations 2
Phase-1 volume fraction = 0.601877 Min(alpha.water) = 1.24552e-07 Max(alpha.water) = 1
MULES: Correcting alpha.water
Phase-1 volume fraction = 0.601877 Min(alpha.water) = 1.14085e-07 Max(alpha.water) = 1
smoothSolver: Solving for Ux, Initial residual = 0.00088217, Final residual = 9.89521e-07, No Iterations 1
smoothSolver: Solving for Uz, Initial residual = 0.000999653, Final residual = 1.9488e-08, No Iterations 2
DICPCG: Solving for p_rgh, Initial residual = 0.0457134, Final residual = 0.000413374, No Iterations 9
time step continuity errors : sum local = 2.82853e-05, global = 1.22492e-16, cumulative = 4.33519e-13
DICPCG: Solving for p_rgh, Initial residual = 0.000763777, Final residual = 7.62554e-06, No Iterations 85
time step continuity errors : sum local = 5.5095e-07, global = 1.22566e-16, cumulative = 4.33641e-13
GAMGPCG: Solving for p_rgh, Initial residual = 2.23129e-05, Final residual = 1.99164e-09, No Iterations 5
time step continuity errors : sum local = 1.34186e-10, global = 1.22444e-16, cumulative = 4.33764e-13
........
PIMPLE: Iteration 8
smoothSolver: Solving for alpha.water, Initial residual = 0.000411351, Final residual = 1.53598e-09, No Iterations 2
Phase-1 volume fraction = 0.601877 Min(alpha.water) = 1.24551e-07 Max(alpha.water) = 1
MULES: Correcting alpha.water
Phase-1 volume fraction = 0.601877 Min(alpha.water) = 1.14317e-07 Max(alpha.water) = 1
smoothSolver: Solving for Ux, Initial residual = 7.20231e-05, Final residual = 8.15403e-08, No Iterations 1
smoothSolver: Solving for Uz, Initial residual = 7.22743e-05, Final residual = 1.58703e-07, No Iterations 1
DICPCG: Solving for p_rgh, Initial residual = 9.49839e-05, Final residual = 9.48353e-07, No Iterations 8
time step continuity errors : sum local = 6.49024e-08, global = 1.22356e-16, cumulative = 4.3609e-13
DICPCG: Solving for p_rgh, Initial residual = 1.46942e-06, Final residual = 1.45553e-08, No Iterations 82
time step continuity errors : sum local = 1.04097e-09, global = 1.2232e-16, cumulative = 4.36212e-13
GAMGPCG: Solving for p_rgh, Initial residual = 4.09335e-08, Final residual = 5.66621e-10, No Iterations 2
time step continuity errors : sum local = 3.93621e-11, global = 1.22389e-16, cumulative = 4.36335e-13
PIMPLE: Converged
Doing final iteration
PIMPLE: Iteration 9
smoothSolver: Solving for alpha.water, Initial residual = 0.000411313, Final residual = 1.53734e-09, No Iterations 2
Phase-1 volume fraction = 0.601877 Min(alpha.water) = 1.24551e-07 Max(alpha.water) = 1
MULES: Correcting alpha.water
Phase-1 volume fraction = 0.601877 Min(alpha.water) = 1.14321e-07 Max(alpha.water) = 1
smoothSolver: Solving for Ux, Initial residual = 0.000171374, Final residual = 7.1472e-07, No Iterations 1
smoothSolver: Solving for Uz, Initial residual = 0.000172324, Final residual = 3.90396e-08, No Iterations 2
DICPCG: Solving for p_rgh, Initial residual = 0.00987837, Final residual = 9.7336e-05, No Iterations 8
time step continuity errors : sum local = 2.21655e-05, global = 1.22798e-16, cumulative = 4.36458e-13
DICPCG: Solving for p_rgh, Initial residual = 0.000297428, Final residual = 2.74392e-06, No Iterations 80
time step continuity errors : sum local = 6.31496e-07, global = 1.22849e-16, cumulative = 4.3658e-13
GAMGPCG: Solving for p_rgh, Initial residual = 2.4488e-05, Final residual = 2.67693e-10, No Iterations 4
time step continuity errors : sum local = 6.332e-11, global = 1.22822e-16, cumulative = 4.36703e-13
PIMPLE: Converged in 9 iterations
ExecutionTime = 34349.1 s ClockTime = 34575 s
End
Finalising parallel run
- run simulation with very small fixed time step - 2nd order time integration - stricter tolerances for outer Iterations "outerCorrectorResidualControl" (did not converge in 100 iterations) ... should I try with 500? - different relaxation factors - turn off momentumPredictor EDIT: Attached complete case for more clarity / providing missing information Any hints on how to proceed would be highly appreciated! Best Regards, Leif Last edited by Leifheit; January 23, 2023 at 05:19. Reason: Attached zip of complete case |
|
|
|
|
|
January 24, 2023, 03:34
|
|
#2 |
|
New Member
Join Date: Jul 2013
Posts: 21
Rep Power: 13 |
Hey everyone,
I made considerable progress, although there is still room for improvement Changing the divergence schemes entries from Code:
divSchemes
{
default none;
div(rhoPhi,U) Gauss vanLeer;
div(phi,alpha) Gauss vanLeer;
div(phirb,alpha) Gauss interfaceCompression;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
to Code:
divSchemes
{
default none;
div(rhoPhi,U) Gauss vanLeer;
div(phi,alpha) Gauss interfaceCompression vanLeer 1;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
resulted in a much cleaner pressure plot, see attachment. Will post updates if further improvement is made. |
|
|
|
|
|
|
|
|
Similar Threads
|
||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| [General] Extracting ParaView Data into Python Arrays | Jeffzda | ParaView | 30 | November 6, 2023 22:00 |
| courant number increases to rather large values | 6863523 | OpenFOAM Running, Solving & CFD | 22 | July 6, 2023 00:48 |
| pimpleDyMFoam computation randomly stops | babapeti | OpenFOAM Running, Solving & CFD | 5 | January 24, 2018 06:28 |
| same geometry,structured and unstructured mesh,different behaviour. | sharonyue | OpenFOAM Running, Solving & CFD | 13 | January 2, 2013 23:40 |
| plot over time | fferroni | OpenFOAM Post-Processing | 7 | June 8, 2012 08:56 |
1Likes
Linear Mode
