Correct pressure distribution but wrong aerodynamics coefficients
 

Hello to everybody.

I have been working with OpenFOAM and I have a strange problem. I have simulated several times a 2D cylinder, with different meshes and solvers and I always obtain a correct pressure and velocity results but a too small drag coefficient. I have calculated it by hand, sampling the pressure over the cylinder, and then the drag coefficient is ok. Where could be the problem?

In literature Cd for a cylinder with our Reynold is about 0.8 but forceCoeffs function calculates 0.3.

This our controlDict file:


---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application simpleFoam;

startFrom latestTime;

startTime 0;

stopAt endTime;

endTime 600;

deltaT 1;

writeControl timeStep;

writeInterval 50;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression uncompressed;

timeFormat general;

timePrecision 6;

runTimeModifiable yes;

functions
(
forceCoeffs
{
type forceCoeffs;
functionObjectLibs ("libforces.so");
//outputControl outputTime;
//outputInterval 1;
outputControl timeStep;
outputInterval 1;
patches (paredes); //change to your patch name
rhoInf 1.225;
CofR (0 0 0);
liftDir (0 0 1);
dragDir (-1 0 0);
pitchAxis (0 0 0);
magUInf -50;
lRef 1;
Aref 1;
}

forces
{
type forces;
functionObjectLibs ("libforces.so"); // Lib to load
//outputControl outputTime;
//outputInterval 1;
outputControl timeStep;
outputInterval 10;
patches (paredes); // change to your patch name
rhoName rhoInf;
rhoInf 1.225; // Reference density for fluid
CofR (0 0 0); // Origin for moment calculations
}

);

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

Any suggestions.

Thank you.

Are you sure of your Aref and lref values? For a 2D cilinder drag calculation in OpenFOAM lref should be the diameter (or the radius if you are simulating only half of the domain) and Aref should be lref*Zmesh, where Zmesh is cells' dimension in the direction orthogonal to your solution domain.

Hope this helps

V.

I'm not sure. But for me this values seem to be strange!
Check them again.
liftDir (0 0 1);
dragDir (-1 0 0);

You defined -x as the direction for the drag and +z for the lift.
Are you sure about them?

Thankyou very much, i didn't know it so I'm going to try!!

Thank you for your coment aut_iut, lift Dir was wrong because I did not want to know it and dragDir is ok because my magUInf is also negative.

Hi aut_iut and Aerospace
I am new user in openFoam and tried with dsmcFoam solver. i need to have aerodynamic coefficient
and i change the controlDict as above but it don't answer
could you help me ?
tanks a lot

Salam Esmaeil,

Could you let me know what kind of error you've got?

regards,

salam dear Rasoul
Tanks for your reply
In fact I saw fallowing warning in log.dsmcfoam file
FOAM Warning :
From function void forces::read(const dictionary&)
in file forces/forces.C at line 277
Could not find U, p in database.
De-activating forces.
best regardes

of course I added the following lines in controlDict file
forceCoeffs1
{
type forceCoeffs;
functionObjectLibs ("libforces.so");
outputControl outputTime;
//outputInterval 1;
//outputControl timeStep;
outputInterval 1;
patches (obstacle); //change to your patch name
pName p;
UNmae U;
log true;
rhoName rhoInf;
rhoInf 1.225;
CofR (0 0 0);
liftDir (0 1 0);
dragDir (1 0 0);
pitchAxis (0 0 0);
magUInf 7600;
lRef 2.5146;
Aref 0.25146;
}

Hi Esmaeil,

It seems that the OpenFOAM can not find U and p files. Be sure that U and p files are available at 0 filder (initial conditions).
Are you using the same name for your patch? I guess you need to change the name of the patch based on your case.
By the way, you should have been added both forcecoeffs and forces at ControlDict file.
Add this:

functions
(
forceCoeffs
{
type forceCoeffs;
functionObjectLibs ("libforces.so");
//outputControl outputTime;
//outputInterval 1;
outputControl timeStep;
outputInterval 1;
patches (paredes); //change to your patch name
rhoInf 1.225;
CofR (0 0 0);
liftDir (0 0 1);
dragDir (-1 0 0);
pitchAxis (0 0 0);
magUInf -50;
lRef 1;
Aref 1;
}

forces
{
type forces;
functionObjectLibs ("libforces.so"); // Lib to load
//outputControl outputTime;
//outputInterval 1;
outputControl timeStep;
outputInterval 10;
patches (paredes); // change to your patch name
rhoName rhoInf;
rhoInf 1.225; // Reference density for fluid
CofR (0 0 0); // Origin for moment calculations
}


If you have some difficulties send me your test case and I will take a look on it.

regards,
Rasoul

Hi dear Rasoul
Thanks fr your suggestions
There is no P and U files in 0 folder in dsmcfoam solver at all !!!
What means of PatchName ?
Best regards.

what`s your Reynolds number and is it suitable to simulate at that Re number by 2D?