CFD Online Discussion Forums - Implementation of the drag coefficient Formula

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Post-Processing (https://www.cfd-online.com/Forums/openfoam-post-processing/)

- - Implementation of the drag coefficient Formula (https://www.cfd-online.com/Forums/openfoam-post-processing/121168-implementation-drag-coefficient-formula.html)

Implementation of the drag coefficient Formula

Hello Foamers :)

I am trying to simulate a flow around a half-cylinder.In order to evaluate my result and i need calculate some coefficients non-dimensional numbers , like Nussel-number and the drag coefficient:

For the calculation of the drag coefficient of the geometry i should use this Formula :

https://rb-owa-portal.emea.bosch.com...8eT5B5WMwMl5LQ
with

https://rb-owa-portal.emea.bosch.com...SIug4AXS5V%2f2

I am using ParaView and Ensight as a Post-Processing Tool.

Can anybody explain to me, how and where should implement this Formula, in order to calculate the drag coefficient for every time step ?

Thx for the support :)

PS: I am using OpenFOAM 2.2.0

So...:)

Just write this Code in your controlDict-File :)

Code:

functions

(

forces

{

type forces;

functionObjectLibs ("libforces.so"); //Lib to load -> dylib on Mac and so on Linux

rhoInf 1.0; //Reference density for fluid - can be changed later ...

patches (fixedWalls); //Name of patche to integrate forces

CofR (0 0 0); //Origin for moment calculations

outputControl timeStep;

outputInterval 1;

}

forceCoeffs

{

// rhoInf - reference density

// CofR - Centre of rotation

// dragDir - Direction of drag coefficient

// liftDir - Direction of lift coefficient

// pitchAxis - Pitching moment axis

// magUinf - free stream velocity magnitude

// lRef - reference length

// Aref - reference area

type forceCoeffs;

functionObjectLibs ("libforces.so");

patches (fixedWalls);

rhoName rhoInf;

rhoInf 1000;

CofR (2 0 0);

liftDir (0 1 0);

dragDir (1 0 0);

pitchAxis (0 0 1);

magUInf 1e-7;

lRef 0.06; // sphere diameter

Aref 0.0014137; //1/2 * projected area = pi*r²/2



        outputControl   timeStep;

        outputInterval  1;

}





);

The Folder postProcessing will be created, there you will find the values of Lift, Drag for every time step saved in the forceCoeffs.dat file :D

For more information :

http://www.cfd-online.com/Forums/ope...efficient.html
http://ww3.cad.de/foren/ubb/Forum527...000069-2.shtml

Hello :)

i did a little mistake :(

The simulation was running and the OpenFOAM calculated the drag , lift....and that is why i thought every is perfect ....

but

i did not calculate the forces properly :

Code:

--> FOAM Warning : 

    From function void forces::read(const dictionary&)

    in file forces/forces.C at line 449

    Could not find U, p or rho in database.

    De-activating forces.

Do you know, how to fix this warning ??

Thx :)

You didn't mention what solver you were using but I think the problem might be that you didn't specify the field names in your controlDict file. Here's how I do it with interFoam and pimpleDyMFoam and it works:

Code:

    forces

    {

        type        forces;

        functionObjectLibs ( "libforces.so" );

        outputControl timeStep;

        outputInterval 1;

        patches

        (

           "hull.*"

        );

        rhoName     rho;        

        pName       p;

        UName       U;

        log         true

        rhoInf      1;

        CofR        (-5.95 -0.518 -0.5705);

    }