[boffin5]

After a bit of effort, I have my aircraft heat exchanger simulation running.
But, the results don't seem to make sense. Attached is an image of the T field,
with some representative air temperatures in front of the HX, and behind it.

As can be seen, the air temperature in front of the HX is 2 degrees hotter than the air temperature behind it. This doesn't make sense, as the heated air should be coming out of the radiator, behind it.

I am attaching some relevant files for those who might be interested, including the p and T files for the fluid and porous zones. Also the constant/fluid/fvOptions file, which defines the porosity of the porous zone.

Note in my simulation, the longitudinal axis is along the Y direction, with the X axis coming out of the screen. This caused me some confusion with the fvOptions e1 and e2 variables. But I think(?) I have it right.

Here is the fvOptions file:

fluidToporous
{
    type            constantHeatTransfer;

    interpolationMethod cellVolumeWeight;
    nbrRegion       porous;
    master          false;

    nbrModel        porousTofluid;
    fields          (h);
    semiImplicit    no;
}

porosityBlockage
{
    type            interRegionExplicitPorositySource;

    interRegionExplicitPorositySourceCoeffs
    {
        interpolationMethod cellVolumeWeight;
        nbrRegion       porous;

        type            DarcyForchheimer;
        
        // D 100;  // Very little blockage
        // D 200;  // Some blockage but steady flow
        // D 500;  // Slight waviness in the far wake
        // D 1000; // Fully shedding behavior

        d   (400  400  100);
        f   (400  400  100);

        coordinateSystem
        {
            origin  (0 0 0);            
            e1      (0 -1 0);    // (0 -1 0)
            e2      (1 0 0);     // (1 0 0)             
            }
        }
    }

The T and p BC files for the fluid zone:

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

dimensions      [0 0 0 1 0 0 0];

internalField   uniform 272.3;

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"
    
    frontier
    {
        type            slip;
    }

    inlet
    {
        type            fixedValue;
        value           uniform 272.3;
    }

    outlet
    {
        type            inletOutlet;
        inletValue      uniform 272.3;
        value           uniform 272.3;
    }

    "fuselage|duct|lips|rad-fairing"
    {
        type            zeroGradient;
    }
    
    centerline
    {
        type            symmetry;
    }
}


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



/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2412                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


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

internalField   uniform 75300;

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"

    inlet
    {
        type            zeroGradient;
    }

    outlet
    {
        type            fixedValue;
        value           $internalField;
    }

    frontier
    {
        type            slip;
    }

    "fuselage|duct|lips|rad-fairing"
    {
        type            zeroGradient;
    }

    centerline
    {
        type            symmetry;
    }
}

And for the porous zone:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2412                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 1 0 0 0];

internalField   uniform 383;

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"
    
    radinlet
    {
        type            fixedValue;
        value           uniform 272.3;
    }

    radoutlet
    {
        type            inletOutlet;
        inletValue      uniform 383;
        value           uniform 383;
    }

    rad_radfrontier
    {
        type            zeroGradient;
    }
    
    rad_radcenterline
    {
        type            symmetry;
        }
}


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


/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2412                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


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

internalField   uniform 75300;

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"

    radinlet
    {
        type            zeroGradient;
    }

    radoutlet
    {
        type            zeroGradient;
        }

    rad_radfrontier
    {
        type            zeroGradient;
    }

   rad_radcenterline
    {
        type            symmetry;
    }

    
}

The ambient air temperature is 272.3 deg K, and for the porous zone T is 383 deg K. The aircraft speed is 84.88 meters per second.

Hopefully with help, I can solve this mystery!

[dlahaye]

No clue, sorry to say.

I, however, wonder.

Does it make sense here to run an adiabatic case (without the solid) and subsequently run a case in which the presence of the solid is modeled using boundary conditions?

[Tobermory]

It looks to me that the rise in temperature upstream of the HX is due to the flow decelerating in the diffuser just upstream of the HX (which, with a compressible equation of state leads to a pressure rise and small temperature rise) ... you can see the same effect, and same deltaT, in other parts of the picture where the flow is decelerating, and the opposite (a cooling) in the nozzle downstream of the HX where the flow is accelerating.

My suspicion is that the HX heat source is not active ...?

[Tobermory]

I am not familiar with prorous zone modelling, or how your two zones interact, but one quick observation on your porous zone boundary:

    radoutlet
    {
        type            inletOutlet;
        inletValue      uniform 383;
        value           uniform 383;
    }

I don't think that this is doing what you think it is. By default, if the flow is exiting the porous zone through this boundary, then the temperature on the boundary will be governed by the temperature of the fluid that enters the boundary ... i.e. the upstream fluid, at 272K. The inletValue of 383K is only used if there is reverse flow INTO the porous zone through the outlet boundary ... which I am assuming is not the case. The "value" part of the boundary is ignored (in fact, if you look at your solution, in the T file you will find that this value has been updated with the latest calculated boundary T value .. which is probably 272K!). This explains why the outlet temperature from the HX is 272K.

So, long and short of it - you can't inject heat into the porous region using an inletOutlet outlet condition ... you need to either do it at the inlet to the porous region, or using a volume source.

Hope that helps.