[cfd_saad]

Hi foamers,

I have been struggling to get the right dynamic pressure from p_rgh. I looked for other subjects dealing with p_rgh and p but I can't found a satisfactory response.

I am studying a cube and I am using interFoam as a solver.

My p_rgh is much higher than p.

I saw in the source file pEqn.H and interFoam.C , that pressures are defined as follow :

p = p_rgh + rho*gh
p_rgh = p - rho*gh

And gh = (g & mesh.C()) - ghRef
with ghRef = (- mag(g)*hRef)

In doxygen manual I found : hRef by default is equal to 0 m

I defined the origin (0 0 0) of my coord system at the bottom so my freesurface is at +32 m.

Do I have to define my coord system's origin at my freesurface or should I create a file hRef in constant folder in which I indicate the height of my freesurface ?

Thanks!!

[Tobermory]

First up, p_rgh is not "dynamic pressure"; dynamic pressure is a measure of the kinetic energy of the flow, . p_rgh is an OpenFOAM construct, that makes some of the equations simpler. It has no real physical meaning, although in incompressible, constant density flows it is equivalent to the deviation from the hydrostatic pressure.

As for where to set hRef - it really doesn't matter. Fluid flow is driven by gradients in p_rgh, and so the absolute value is unimportant (by contrast, the absolute value of p can be important, eg for defining density in vapour flows, but again that is not affected by hRef). Simplest, though, is to set hRef to a value that sets p_rgh for the majority of the domain to be close to zero ... and that would mean setting it at the free surface. Do that with a constant/hRef file, as you noted.

[cfd_saad]

Excellent! I did put hRef value at my free surface, now I have the right pressure value without the hydrostatic pressure for p_rgh.

But for the incompressible flows, we can call p_rgh the dynamic pressure ? since only dynamic components are taken into account.

[cfd_saad]

Here is the file hRef, for those interested :

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       uniformDimensionedScalarField;
    location    "constant";
    object      hRef;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 0 0 0 0 0];
value           32;

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

[buesinaw]

So if one gets a p_rgh value from a probe location (x y z) defined in the controlDict, is that p_rgh value for that exact (x y z) location or is it the p_rgh value for the mesh.C() location nearest to the probe location (x y z)?

[Tobermory]

I think that by default it interpolates the cell centre values to the probe location ... may have that wrong; suggest you test it.

You can control whether it interpolates or just uses the nearest cell centre with the interpolationScheme parameter - check out for example:

https://www.openfoam.com/documentati...#x30-1330007.4

[buesinaw]

You're correct, I should test it. Sorry that I haven't, I will, but thank you for your reply.

How would one get the coordinates of the center of the cell in which the probe is located?

[Tobermory]

As a test, if you know what the approximate cell size is, D, then you can just put in say 10 probes, spaced D/5 apart and then see whether the results you get from the 10 probes follow a linear profile or a staircase profile as they traverse the 2 or 3 cells.