[nainavinod]

Hello Foamers,

I am currently running a large overset mesh case (~40 million cells) to simulate a propeller rotating at a certain rpm. The set-up is very similar to the "simpleRotor" tutorial case, except I have a more well defined propeller geometry. It uses the incompressible overPimpleDyMFoam solver.

I am trying to extract the surface pressure distribution on the propeller and I use the surface sampling library for it as shown below:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F yield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2006                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

surfaces
{
    type            surfaces;
    libs            (sampling);
    timeStart       0.429997;
    timeEnd         0.489997;
    writeControl    timeStep;
    writeInterval   4;
    surfaceFormat   ensight;
    fields          (p wallShearStress);

    interpolationScheme cellPoint;  //<- default

    surfaces
    {
        propeller
        {
            type            patch;
            patches         ("Propeller");
            interpolate     false;
            //invariant       true;  // Unaffected by mesh motion
            //fixedLocations  false;
            surfaceFormat   ensight;
        }
    }
}


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

I dont believe the surface sampling for overset meshes works correctly on OpenFOAM. And here's my reasoning:

- I did a simple check to ensure the sampled surface data is correct or not. (Data obtained from : $CASE_DIR/postProcessing/surfaces/propeller/propeller.case). I calculated the integrated thrust (integral of the quantity: p*Normal_Z-wallShearStressZ) on Paraview for a particular time instance.
- I compared the thrust value I got from Paraview with the value predicted by the libforces library for the same time instance. They do not match and vary by a very large margin(~20% error).
- I tried switching the interpolation "on" and "off" while using the surface sampling library and that didn't affect the solution either.

This made me check one of the reconstructed time files as well. I opened it on Paraview and calculated the integrated thrust over the propeller surface. This matched the value predicted by the surface sampling and obviously did not agree with the value predicted by libforces.

I have reason to trust the value predicted by libforces as it is in line with past literature and experimental data. However, the surface sampling library and the recontructed files are underpredicting surface pressure. If someone has faced this problem, or knows how to fix it, please let me know. I have been stuck with the issue for a while now.

[Yann]

Hi,

Incompressible solvers in OpenFOAM use kinematic pressure. (https://www.openfoam.com/documentati...-pressure.html)

You have to multiply p by the density to get the static pressure if you want to compute forces in paraView. This is already handled in libforces since you need to define rhoInf in the function definition.

If you are working with air, this might explain the 20% error.

I hope this helps,
Yann

[nainavinod]

Hey Yann!

That actually makes complete sense. I knew this about incompressible solvers but it completely slipped out of my head when I was trying to calculate the forces. I added the density factor and now the solution is spot on. Thank you so much. This was very helpful.

Thank You,
Naina.