[mump0]

Hi all!

I'm solving a compressor with rhoporousmrfsimplefoam and my problem is,that my real total enthalpy is below the isentrope one at the outlet. So i have an efficieny factor above 1(what a nice factor ), but it should be near by 0.7(CFX). At the outlet my pressure is near by the value of CFX(a little bit to high), total temperature is to low and my density is to high. To find my mistake much faster i created a case with a simple pipe and the same settings and solver. I changed some BC's and other settings, but there is still the same problem. When i solve it laminar with low velocity the result looks fine. Is there a problem with my komegasst-model? Or maybe my BC's are not correct?
These are the files of the pipe-case:

p:

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 1.0133e5;
boundaryField
{
OUTLET
{
type zeroGradient;
}
WALL
{
type zeroGradient;
}
INLET
{
type totalPressure;
U U;
psi psi;
phi phi;
gamma 1.4;
p0 uniform 1.0133e5;
value uniform 1.0133e5;
}
}
// ************************************************** *********************** //

U:

FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
OUTLET
{
type flowRateInletVelocity;
flowRate -0.2;
value uniform (0 0 0);
}
WALL
{
type fixedValue;
value uniform (0 0 0);
}
INLET
{
type zeroGradient;
}
}
// ************************************************** *********************** //

T:

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
internalField uniform 298.15;
boundaryField
{
OUTLET
{
type zeroGradient;
}
INLET
{
type totalTemperature;
U U;
psi psi;
phi phi;
gamma 1.4;
T0 uniform 298.15;
value uniform 298.15;
}
WALL
{
type zeroGradient;
}
}
// ************************************************** *********************** //

k:

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 1;
boundaryField
{
OUTLET
{
type zeroGradient;
}
INLET
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.05;
value uniform 1;
}
WALL
{
type compressible::kqRWallFunction;
value uniform 1;
}
}

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

omega:

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 -1 0 0 0 0];
internalField uniform 500;
boundaryField
{
OUTLET
{
type zeroGradient;
}
INLET
{
type fixedValue;
value uniform 500;
}
WALL
{
type compressible:megaWallFunction;
value uniform 500;
}
}

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

alphat and mut are default.

Does someone has any idea?

Regards, Eric

[mump0]

edit: In the case with the simple pipe the total temperature at the outlet is lower than the total temperature at the inlet, but it should be the same, because its adiabatic. I think my BC's are correct, aren't they? So is there a problem with the h-equation or something else?

Thank you in advance!

Regards, Eric

[dre]

I encountered a similar issue. I was simulating a compressor wheel with rhoPorousMRFSimpleFoam using OpenFOAM 2.1.x. Despite compression, the temperature decreased by about 30K. Previous simulations with openFOAM 2.0.x resulted in an increase of about 30K.

So I took a closer look at the hEqn.H of the solver:

OpenFOAM 2.1.x

    fvScalarMatrix hEqn
    (
        fvm::div(phi, h)
      - fvm::Sp(fvc::div(phi), h)
      - fvm::laplacian(turbulence->alphaEff(), h)
     ==
      - fvc::div(phi, 0.5*magSqr(U), "div(phi,K)")
    );

OpenFOAM 2.0.x

    fvScalarMatrix hEqn
    (
        fvm::div(phi, h)
      - fvm::Sp(fvc::div(phi), h)
      - fvm::laplacian(turbulence->alphaEff(), h)
     ==
        fvc::div(phi/fvc::interpolate(rho), rho/psi, "div(U,p)")
      - (rho/psi)*fvc::div(phi/fvc::interpolate(rho))
    );

So there has been a change in the enthalpy equation. However, I don't know the reason for that. Can someone help to clarify this?

[prasant]

Hello All,

Did you get any information regarding correction in hEqn If so, please share the information with me. I tried to modified the hEqn as per Eric comments. But still outlet temperature is decreasing.

Regards
Prasant.