[Sugajen]

Hi all,

I am trying to run a pressure driven flow simulation using reactingTwoPhaseEulerFoam. I get an error when I specify totalPressure in inlet p_rgh.

--> FOAM FATAL ERROR: 

    request for volVectorField U from objectRegistry region0 failed
    available objects of type volVectorField are

6
(
U.particles_0
DUDt.particles
U.air
U.air_0
U.particles
DUDt.air
)


    From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&) const [with Type = Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>]
    in file /home/ubuntu/OpenFOAM/OpenFOAM-4.1/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 193.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const at ??:?
#3  Foam::totalPressureFvPatchScalarField::updateCoeffs() at ??:?
#4  Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/reactingTwoPhaseEulerFoam"
#5  Foam::fv::EulerDdtScheme<double>::fvmDdt(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:?
#6  Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::ddt<double>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/reactingTwoPhaseEulerFoam"
#7  ? in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/reactingTwoPhaseEulerFoam"
#8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9  ? in "/opt/openfoam4/platforms/linux64GccDPInt32Opt/bin/reactingTwoPhaseEulerFoam"
Aborted (core dumped)

For fixedValue inlet p_prgh, the velocties keep increasing with each time step and does not make sense.
When I used the totalPressuere in inlet P instead of p_rgh, I get reasonable values, but that is not the right way to do, right ?
I searched the forum for relevant threads, but none touched this explicitly, and hence the post.
I am attaching my p, p_rgh and U files below.
P:

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 1.04e5;

boundaryField
{

    inlet
    {
	type		calculated;
	value		$internalField;
    }

    outlet
    {
	type		calculated;
	value		$internalField;
    }

    top
    {
	type		calculated;
	value		$internalField;
    }

    bottom
    {
	type		calculated;
	value		$internalField;
    }

    walls
    {
	type		calculated;
	value		$internalField;
    }

    frontAndBack
    {
        type		empty;
    }

p_rgh:

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 1.04e5;

boundaryField
{

    inlet
    {
	type            totalPressure;
	p0              $internalField;
	value           $internalField;
    }

    outlet
    {
	type 		prghPressure;
	p 		uniform 0;
    }

    top
    {
        type		fixedFluxPressure;
        value    	$internalField;
    }

    bottom
    {
        type		fixedFluxPressure;
        value    	$internalField;
    }

    walls
    {
        type 		fixedFluxPressure;
        value 		$internalField;
    }

    frontAndBack
    {
        type            empty;
    }
}

U:

FoamFile
{
    version     2.0;
    format      binary;
    class       volVectorField;
    location    "0";
    object      U.air;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform (0.0 0.0 0.0);

boundaryField
{

    inlet
    {
        type            fixedValue;
	value		$internalField;
    }

    outlet
    {
        type            fixedValue;
	value		$internalField;
    }

    top
    {
        type            noSlip;
    }

    bottom
    {
        type            noSlip;
    }

    walls
    {
        type            noSlip;
    }

    frontAndBack
    {
        type            empty;
    }

}

Any comments, suggestions or guidance will be greatly appreciated.
Thanks in advance

Sugajen

[jaydeep]

Your error is pretty self explanatory. You can look for the boundary definition here:
https://github.com/OpenFOAM/OpenFOAM...hScalarField.H

You will find that the boundary does calculation along the lines of:

            p_p = p_0 - 0.5 |U|^2

So it needs "U" field. In your case, you will need to explicitly feed U field for species. The definition is given in the same source file:

Usage
        Property     | Description                | Required | Default value
        U            | Velocity field name        | no       | U
        phi          | Flux field name            | no       | phi
        rho          | Density field name         | no       | rho
        psi          | Compressibility field name | no       | none
        gamma        | (Cp/Cv)                    | no       | 1
        p0           | Total pressure             | yes      |

[sjohn2]

Hi,

I have the same problem. I want to specify total pressure in the inlet and static pressure in the outlet using the same solver reactingtwophaseeulerFoam. Does any one have an example?