[CFDnewbie147]

Hello together,

I have some questions on OpenFoam. I've converted a TAU- Mesh into the OF format via Fluent and with TAU we use two spheres to define the near- and farfield around the geometry. We are defining the machnumber and the temperature and pressure and the incoming velocity vectors are all parallel to the flight direction.

My question is: is it possible to define a sphere(farfield) for inlet and outlet in openfoam or have there to be always two faces, one for inlet and one for outlet, like building a mesh via blockmesh?

I hope u know what I mean and you can help me.
Best regards,
CFDNEWBIE147

[henrik]

Dear CFDNEWBIE147,

rather than splitting the patch, I suggest that you use a boundary condition which switched automatically from fixedValue to zeroGradient based on the flux.

0/U:

inlet
{
type inletOutlet;
inletValue uniform (1 1 0);
value uniform (1 1 0);
}

0/p:

pressure-far-field-1
{
type zeroGradient;
}

Don't forget to apply inletOutlet on other variables (k, epsilon) in the same manner.

Best Regards,

Henrik

[CFDnewbie147]

Dear henrik,

thank you for your reply. If I change the 0/U to what you've said, there's an error that OF wants a scalar and not a vector...

What's wrong about this?

And can you please explain, how to apply inletOutlet on the other variables? I don't really know how to do this...

I hope you can help me again.
Best regards,
CFDnewbie147

[henrik]

Hard to say without further information. The error is probably what OpenFOAM says: It needs a vector "(1 0 0)", but it found a scalar "1". Please post the full error message line and the part of the input that OF is referring to in that message.

[skyinventorbt]

Originally Posted by CFDnewbie147

Dear henrik,

thank you for your reply. If I change the 0/U to what you've said, there's an error that OF wants a scalar and not a vector...

What's wrong about this?

And can you please explain, how to apply inletOutlet on the other variables? I don't really know how to do this...

I hope you can help me again.
Best regards,
CFDnewbie147

For example you must have used
inletValue uniform (0 0 0);
instead of
inletValue uniform 0:

--
KANNAN

[AndreasG]

In addition to Henriks comment, I would suggest to use outletInlet for the pressure on the farfield where you use inletOutlet for the velocity.

Based on the flux, those two bc switch between Neumann and Dirichlet type.
inletOutlet is fixed value for inflow and zero gradient for outflow (what Henrik suggested for velocity and the other parameters)
outletInlet is the other way round, so it is zero gradient when flux is pointing into the domain and fixed value when the flow is going out of the domain.

so, for 0/p in an incompressible flow:
inlet
{
type outletInlet;
outletValue uniform 0; // the fixed value, when it is an outlet
value uniform 0; // current value (initial guess), will be updated where the flow is into domain
}

[CFDnewbie147]

Hello again,

Here is my polyMesh/boundary file:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       polyBoundaryMesh;
    location    "constant/polyMesh";
    object      boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
8
(
    B_11
    {
        type            wall;
 inGroups 1(GeoWallGroup);
        nFaces          540;
        startFace       17381367;
    }
    B_10
    {
        type            wall;
 inGroups 1(GeoWallGroup);
        nFaces          7602;
        startFace       17381907;
    }
    B_13
    {
        type            wall;
 inGroups 1(GeoWallGroup);
        nFaces          4284;
        startFace       17389509;
    }
    B_12
    {
        type            wall;
 inGroups 1(GeoWallGroup);
        nFaces          24550;
        startFace       17393793;
    }
    B_2//Farfield
    {
        type            patch;
        nFaces          1442;
        startFace       17418343;
    }
    B_4
    {
        type            wall;
 inGroups 1(GeoWallGroup);
        nFaces          26742;
        startFace       17419785;
    }
    B_6
    {
        type            wall;
 inGroups 1(GeoWallGroup);
        nFaces          7286;
        startFace       17446527;
    }
    B_8
    {
        type            wall;
 inGroups 1(GeoWallGroup);
        nFaces          2450;
        startFace       17453813;
    }
)
// ************************************************************************* //

There is my B_2 = Farfield that should be my in- and outlet. I think you don't know exactly what I mean or am I wrong?

And this is my 0/U file, which i adopted to what you've said:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 1 -1 0 0 0 0];
internalField   uniform (50 0 0);
boundaryField
{
    B_2
    {
        type            inletOutlet;
 inletValue  uniform (1 1 0);
 value   uniform (1 1 0);
    }
    }
    GeoWallGroup
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
   
}
// ************************************************************************* //

Is this right or did I some failures? And what do I have to do with the other files in 0/*?

I hope you can help me,
CFDnewbie147

[AndreasG]

There is one and maybe a second error:
There is one red curly bracket, which shouldn't be there, as boundaryField {...} should be closed after GeoWallGroup{...}.
The maybe-error is the difference in the values for internalField and inletValue. I guess, the flow velocity is 50 m/s in x-wise direction, so you should set both, value and inletValue to (50 0 0). But thats only a guess ;-)

internalField   uniform (50 0 0);
boundaryField
{
    B_2
    {
        type            inletOutlet;
        inletValue  uniform (1 1 0);
        value   uniform (1 1 0);
    }
    }
    GeoWallGroup
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
}

To your second question:
As Henrik and me wrote above, use inletOutlet for U and other fields like turbulence parameters, temperature, density, etc. on the farfield.
For the pressure I would use outletInlet for the pressure

inlet
    {
        type outletInlet;
        outletValue     uniform 0; // the fixed value, when it is an outlet
        value           uniform 0; // current value (initial guess), will be updated where the flow is into domain
    }

[henrik]

I agree:

- the 'red' bracket is definitely wrong
- the different values will slow down convergence, but the BC will win.
- Other variables are k, epsilon, omega, ... treat like velocity (so inletOutlet), but with a sensible scalar value
- outletInlet on p - yes, another option - Should not be very different

Additional comments:

You may want to use $internalField in the BC. See

$FOAM_TUT/compressible/rhoPimpleFoam/angledDuct/0/T

None of this explains the error message which you are reporting. If it prevails, please post the complete message together with the relevant sections of the file it refers to.

Ah, and pressure should be 100000 in case you are running a variable density solver.

[CFDnewbie147]

Hello again,

thank you for your answers. I will try what you've said and post what's going on with the simulation.

Best regards,
CFDNewbie147

[CFDnewbie147]

Back again.

It worked, but not as I would it should work. Here are my 0/ files:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 1 -1 0 0 0 0];
internalField   uniform (50 0 0);
boundaryField
{
    B_2
    {
        type            inletOutlet;
 inletValue  uniform (50 0 0);
 value   uniform (50 0 0);
    }

    GeoWallGroup
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
   
}
// ************************************************************************* //

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 2 -2 0 0 0 0];
internalField   uniform 100000;
boundaryField
{
    B_2
    {
        type           outletInlet;
 outletValue uniform 100000;
 value  uniform 100000;
    }
    GeoWallGroup
    {
        type            zeroGradient;
    }
}
// ************************************************************************* //

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      nuTilda;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 2 -1 0 0 0 0];
internalField   uniform 0.14;
boundaryField
{
    B_2
    {
        type            inletOutlet;
 inletValue uniform 0.14;
 value  uniform 0.14;
    }
    GeoWallGroup
    {
        type            fixedValue;
        value           uniform 0;
    }
}
// ************************************************************************* //

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 2 -1 0 0 0 0];
internalField   uniform 0.14;
boundaryField
{
    B_2
    {
        type            inletOutlet;
 inletValue uniform 0.14;
 value  uniform 0.14;
    }

    GeoWallGroup
    {
        type            nutUSpaldingWallFunction;
        value           uniform 0;
    }
}
// ************************************************************************* //

I guess I did what you've said but it doesn't work correctly.
I think I have to fix the direction of the velocity with a main vector with 50m/s only in x- direction?

How can I do this?
Hope you can help again,
best regards,
CFDNewbie147