CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Simulation of a fluidic oscillator with SA-IDDES: oscillation frequency too high

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   April 4, 2017, 03:57
Default Simulation of a fluidic oscillator with SA-IDDES: oscillation frequency too high
  #1
New Member
 
Hendrik
Join Date: Jan 2017
Posts: 2
Rep Power: 0
Zymorui is on a distinguished road
Dear Foamers,
I'm conducting a transient study of a fluidic oscillator with water at 20C (corresponding to nu=1.004e-6). For this I'm using the SpalartAllmarasIDDES turbulence model and the pisoFoam-solver. The Mean Courant Number is 0.1 and the maximum about 7. I average the pressure over a diameter slice in each feedback loop and use the pressure difference between both to calculate a sinoid signal containing the oscillation frequency of the jet for the particular inlet velocity.

My problem is that the CFD oscillation frequency of the jet is almost the double of experimental values. The problem persists for all flow rates even in the laminar regime (where I used no turbulence model). As I have double checked the geometry, the Mesh should be fine (checkMesh):
- 1mio Cells
- blockMesh generated
- y+=1
- cell-to-cell-exp-ratio at the wall is about 1.2
- Non-Ortho-Max 58
- Max aspect ratio 152
- Max skewness 1.7

So I guess there must be something wrong with my fvSchemes or fvSolutions. Does anyone have suggestions what part of the simulation could make the oscillation frequency getting over estimated that strong?

Kind regards,
Hendrik


fvSchemes
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default backward;
}

d2dt2Schemes
{
}

gradSchemes
{
    default         cellLimited Gauss linear 1; //Gauss linear;

    //grad(nuTilda)   cellLimited Gauss linear 1;
    //grad(U)         cellLimited Gauss linear 1;
}

divSchemes	// convection
{
    default         none;

    div(phi,U)      Gauss linearUpwind grad(U); // LUST unlimitedGrad(U);
    div(phi,k)      Gauss limitedLinear 1;
    div(phi,nuTilda) Gauss limitedLinear 1;

    div((nuEff*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes   // diffusion
{
    default         Gauss linear limited corrected 0.33;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         limited corrected 0.33;
}

wallDist
{
    method meshWave;
}


// ************************************************************************* //
fvSolution
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver          GAMG;
        tolerance       1e-5;
        relTol          0.05;
        smoother        GaussSeidel;
	//nSweeps			1;
	nPreSweeps		0;
	nPostSweeps		2;
	nFinestSweeps		2;
        nCellsInCoarsestLevel 50;
	//maxIter			50;
    }

    pFinal
    {
        $p;
	tolerance       1e-5;
        relTol          0;
	//maxIter		100;
    }

    "(U|k|B|nuTilda)"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
	nSweeps		1;
        tolerance       1e-5;
        relTol          0;
    }
}

PISO
{
    nCorrectors     3;
    nNonOrthogonalCorrectors 1;
}

relaxationFactors
{
	p	1;
    "U.*"               1;
    "nuTilda.*"         1;
}


// ************************************************************************* //
Zymorui is offline   Reply With Quote

Old   April 4, 2017, 07:40
Default
  #2
New Member
 
Join Date: Mar 2015
Posts: 14
Rep Power: 4
sati is on a distinguished road
Hi,

A Courant number of 7 is way too high. You should decrease your time step to reach a maxCo < 1.

Last edited by sati; April 5, 2017 at 04:16.
sati is offline   Reply With Quote

Old   April 11, 2017, 03:58
Default
  #3
New Member
 
Hendrik
Join Date: Jan 2017
Posts: 2
Rep Power: 0
Zymorui is on a distinguished road
It took me some time but I've narrowed the issue down to the outlet boundary condition. I did a quick run with fluent and got the right frequency right away. (transient kOmega simulation). But fluent gave the 'A wall has been set at portions of an outlet'-notice. My fixedValue=0 pressure condition at the outlet created backflow, as the vortice cores in the outlet channel were at p<0.

I experimented with advective -> phi, BC for velocity and fixedMean for pressure but it's not quite right yet.

Does anyone have some experience with the backflow issue? Is there a BC that does something similar as fluent does?
Zymorui is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
simulation of airfoil at high AOA hsnu84053 FLUENT 0 January 26, 2007 22:34
Reasons for failed validation at high frequency zonexo Main CFD Forum 5 October 23, 2006 09:32
Airfoil simulation in High Angles of Attack Yasser Nabavi FLUENT 0 April 21, 2006 17:28
MRF simulation : continuity residual high as 0.4 guru FLUENT 2 February 7, 2005 10:33
Problem about 3D blunt body high Re simulation David FLUENT 0 September 27, 2002 10:59


All times are GMT -4. The time now is 15:06.