[edomalley1]

Hi -



I've noticed an interesting issue - when I use OpenFoam to do runtime drag force calculations, they are different than when I calculate them in Paraview. At the same time step, OpenFoam calculates the force to be 2.28N and Paraview gets 1.83N.


In Paraview, after loading the case I do Extract Block on the geometry, then Extract Surface, then Generate Surface Normals, including cell normals. Then Calculator using cell normals, p*Normals_X, then Integrate Variables and display the Cell Normals attribute.


In OpenFoam, here is my forcesIncompressible file. This is a Spalart-Allmaras DDES simulation using pisoFoam. Any idea what is going on and which one (if any) is accurate?

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
-------------------------------------------------------------------------------
Description
    Calculates pressure and viscous forces over specified patches for a case
    where the solver is incompressible (pressure is kinematic, e.g. m^2/s^2).

\*---------------------------------------------------------------------------*/

#includeEtc "caseDicts/postProcessing/forces/forcesIncompressible.cfg"

rhoInf      1.225;    // Fluid density
patches     (Shoe1);
outputControl timeStep;
outputInterval 250;
CofR        (0.03 0 0.03);
pitchAxis   (0 1 0);

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

[simrego]

Hi!


OF calculates the viscous forces too. But I think in paraview you miss this component.

[edomalley1]

Originally Posted by simrego

Hi!


OF calculates the viscous forces too. But I think in paraview you miss this component.

That's true but OF breaks out viscous forces separately from pressure forces. I'm comparing just pressure forces in the x direction.

[Yann]

Hello,

pisoFoam, as many other incompressible solvers is based on the kinematic pressure, which is basically the pressure normalized by density:



You can make sure of that by checking the pressure dimensions in the p file. It should be either m2/s2 if the solver use kinematic pressure or kg/(m.s2) for regular pressure.
E.g in pisoFoam:

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

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

When post-processing in paraview, you need to calculate p*rhoInf to get the actual pressure value.
Using the example you gave in your initial post, it would be something like 1.83*1.225=2.24N, which is closer to what openFoam computes.

I don't know what can cause the remaining difference. Write precision ? Interpolation somewhere in the process ? For such thing I usually just load the patch(es) I want to work with in paraView so I don't use extract block and extract surface filters.

[edomalley1]

Great, thanks!