[L1011]

Hi Foamers!

In the past days I tried to set the case of a simple 2D-incompressible simulation of an airfoil using a O-mesh with the influence of both viscosity and turbulence (SST model) using pisoFoam.

As shown on the figure below, the topology of my case is made of:

1. a body
2. an internal field
3. an inlet/outlet

on which I have to set boundary conditions; basically a freestream velocity vector and an adiabatic/no-splip boundary at wall.

Based on searches in the forum I have 3 questions for you:

A) In the 0/ folder, why do we need to set boundary conditions for all the working variables on all the boundaries? (For example, at wall, couldn't we just set the velocity to 0 instead of adding also a BC for the pressure ?)

B) How can I set non-reflecting boundary conditions for the farfield?

C) Based on my experience, I tried the boundary conditions mentioned hereafter. The computation ran properly but I do not get the right cp distribution nor aerodynamic coefficient values. Did I make a major mistake?

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.4.1                                 |
|   \\  /    A nd           | Web:      http://www.openfoam.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

// Field Dictionary

FoamFile
{
    version         2.0;
    format          ascii;

    root            "";
    case            "";
    instance        "";
    local           "";

    class           volVectorField;
    object          U;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (25 0 0);

boundaryField
{
    inlet-outlet
    {
        type            fixedValue;
        value           uniform (25 0 0);
    }

    body            
    {
        type            fixedValue;
    value           uniform (0 0 0)
    }

    defaultFaces    
    {
        type            empty;
    }
}


// ************************************************************************* //

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.4.1                                 |
|   \\  /    A nd           | Web:      http://www.openfoam.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

// Field Dictionary

FoamFile
{
    version         2.0;
    format          ascii;

    root            "";
    case            "";
    instance        "";
    local           "";

    class           volScalarField;
    object          p;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 82714;

boundaryField
{
    inlet-outlet
    {
        type            zeroGradient;
    }

    body            
    {
        type            zeroGradient;
    }

    defaultFaces    
    {
        type            empty;
    }
}


// ************************************************************************* //

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 0.001;

boundaryField
{
    inlet-outlet
    {
        type            fixedValue;
        value           uniform 0.001;
    }
    body
    {
        type            zeroGradient;
    }
    defaultFaces
    {
        type            empty;
    }
}


// ************************************************************************* //

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      mut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -1 0 0 0 0];

internalField   uniform 0;


boundaryField
{
    inlet-outlet
    {
        type            calculated;
        value           uniform 0;
    }

    body            
    {
        type            mutLowReWallFunction;
        Cmu             0.09;
        kappa           0.41;
        E               9.8;
        value           uniform 0;
    }

    defaultFaces    
    {
        type            empty;
    }
}



// ************************************************************************* //

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volSymmTensorField;
    object      R;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform (0 0 0 0 0 0);

boundaryField
{
    inlet-outlet   
    {
        type            kqRWallFunction;
        value           uniform ( 0 0 0 0 0 0 );
    }

    body
    {
        type            kqRWallFunction;
        value           uniform ( 0 0 0 0 0 0 );
    }

   defaultFaces 
    {
        type            empty;
    }
}

// ************************************************************************* //

Thank you very much and have a good week!

L1011

[olivierG]

Hello,

A) There is not "default condition" in OF, so you must set boundary condition for all variables.

B)
1) For airfoil simulation, first rule is to set your far field domain to 30 - 50 chord lenght. From your picture, you are at 2 only, and you will have big reflexion and distorsion in the u and p field.

2) Your boundary conditions are not optimal. Try:
For U, at inlet-outlet, try the inletOutlet condition
For p, at inlet-outlet, try outletInlet
For k, at inlet-outlet: inletOutlet, and for your wall: fixedValue if y+<1 or kqRWallFunction if y+>30
For omega (if kw SST), the same, i.e inletOutlet and omegaWallFunction at wall.
For mut, seem ok if you use a low Re turbulence model (kw SST is not a low Re model), or mutWallFunction
For R, at inlet-outlet you should try inletOutlet too.

FvScheme: don't forget to use Gauss upwind for div scheme with k/epsilon/omega at first.
FvSolution: set tolerance for omega/k/epsion to a low value , i.e 1e-15, and play with relTol (start at 0.1 to ...1e-6)

Hope this help
olivier

[L1011]

Hi Olivier,

Thank you for your hints, I'll try to make a comparative study with the results already get.

L1011

[VSass]

OivierG,

your post was very helpful to me also,but i want to ask if there is any specific reason or criteria for using outletInlet for p and not inletOutlet?
The same question occurs for velocity.How do we choose one or the other?

[olivierG]

hello,

outletInlet use zeroGradient in case of inflow, and fixedValue for outflow,
inletOutlet use fixedValue for inflow, and zeroGradient for outflow,
so you see that you will use inletOutlet for U at both inlet & outlet, and outletInlet for p (inlet & outlet).
You may try the opposite (i.e use a fixed outflow velocity), but this is realy not a good idea.

regards,
olivier

[sh.d]

Hi
I want simulate a supercritical airfoil by using rhosimplecfoam.mach number is 0.5.but, I do not know what boundary conditions should I use?
pleas help me?