[Gimlas]

I am totally confused with the hydrostatic pressure calculations in openfoam. I've prepared a simulation of air flow through a vertical pipe (buoyantBoussinesqSimpleFoam). I've used following BC for pressures:

p

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    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 0;

boundaryField
{
    Wall
    {
        type            calculated;
        value           $internalField;
    }
    Inlet
    {
        type            calculated;
        value           $internalField;
    }
    Outlet
    {
        type            fixedMean;
        meanValue       0;
    value        uniform 0;
       
    }
}

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

p_rgh

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 0;

boundaryField
{
    Wall
    {
        type            fixedFluxPressure;
        rho             rhok;
        value           $internalField;
    }

    Inlet
    {
        type            fixedFluxPressure;
        rho             rhok;
        value           $internalField;
    }
    Outlet
    {
        type            fixedMean;
        meanValue       0;
    value        uniform 0;
    }
}

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

p_rgh profile is identical to the results obtained from Ansys Fluent (please see attached image). However the p profile is wrong. Althouth uniform 0 value was set at the Outlet, the results show high undepressure. I've made my own calculations using calculator filter in paraView (see p_calculated image). The profile was obtained as follows:

p = p_rgh+(H-coordsY)*9.81*1.225
where H is the pipe height, 9.81 is gravity and 1.225 is air density

As you can see this profile is correct.

My qestion is: why the original p calculations went so wrong? Is there a mistake in the BC?

I've also tried to run calculations without p file in 0 folder. But in next iterations such file was created with incorect pressure field.

Please, help me

[tomf]

Dear Gimlas,

buoyantBoussinesqSimpleFoam is an incompressible solver, meaning that it solves for kinematic pressure, in this case corrected for hydrostatic pressure. This means that the actual pressure value is irrelevant, it is only the gradient that needs to be correct. If you compare your calculated p with the p from buoyantBoussinesqSimpleFoam you see the same gradient, except the calculated one has a density factor for the hydrostatic part, which should not be there, since p_rgh is in fact the kinematic pressure (p_rgh/rho). So you can subtract any value from p in paraview to make sure it is zero at the outlet, or equivalently move you outlet to z=0 and rerun the simulation. The gradient should not be different.

Regards,
Tom

[Gimlas]

Dear tomf,

Of course you're right with the density in the calculated pressure. All calculations are based on the kinematic pressure (m^2/s^2) therefore the correct equation is p_calc = p_rgh+(H-coordsY)*g.

But I'm not sure if I understand you correctly: in order to receive both p and p_rgh pressures equal to 0 I would have to move the whole domain towards -Y axis (vertical one) in order to place the outlet patch at 0 m? If yes, is there an another way to achieve that changing BCs or solution settings? I've tried to change the pressure reference point but it didn't work.

[tomf]

Well you can just add any pressure value to the p or p_rgh value, it does not matter for the solution of your problem (the flow or temperature will not change). This is because only the pressure gradient is important, not it's actual value.

In this case the difference between the pressure p and p_rgh at the outlet is only a consequence of the y-coordinate of your outlet, following your formula. The reference point for the pressure is only used in case of a closed domain (no inlet or outlet), so it makes sense that nothing changed there.

Hope this clarifies my point.
Tom