[DLC]

Hello Everyone!

I'm testing simpleFoam (OF 1.7) on the classic NACA 0012. To obtain forces on the airfoil I use the following commands in the controlDict:

functions
(
forces
{
type forces;
functionObjectLibs ("libforces.so"); //Lib to load
patches (wing); // change to your patch name
rhoInf 1.225; //Reference density for fluid
CofR (0.15 0 0); //Origin for moment calculations
outputControl outputTime;
}
forceCoeffs
{
type forceCoeffs;
functionObjectLibs ("libforces.so");
patches (wing); //change to your patch name
rhoInf 1.225;
CofR (0 0 0);
liftDir (0 1 0);
dragDir (1 0 0);
pitchAxis (0 0 0);
magUInf 55.5;
lRef 0.6;
Aref 1;
outputControl outputTime;
}
);




When I launch the run, this warning message is given and no forces/forces.dat is made (the run goes without any problem)
the same commands work perfectly on interFoam..

can anyone help me?
thanks!

Starting time loop

--> FOAM Warning :
From function void forces::read(const dictionary& dict)
in file forces/forces.C at line 277
Could not find U, p or rho in database.
De-activating forces.
--> FOAM Warning :
From function void forces::read(const dictionary& dict)
in file forces/forces.C at line 277
Could not find U, p or rho in database.
De-activating forces.
Time = 1

[philippose]

Hi,

A Good Morning to you :-)!

You are getting this warning, and the force calculations are subsequently disabled because you are missing one line in your forces function definition... you need to change your function definition to:

functions
(
     forces
     {
         type forces;
         functionObjectLibs ("libforces.so"); //Lib to load
         patches (wing); // change to your patch name
         rhoInf 1.225; //Reference density for fluid
           rhoName rhoInf;
         CofR (0.15 0 0); //Origin for moment calculations
         outputControl outputTime;
     }
     forceCoeffs
     {
         type forceCoeffs;
         functionObjectLibs ("libforces.so");
         patches (wing); //change to your patch name
         rhoInf 1.225;
           rhoName rhoInf;  
         CofR (0 0 0);
         liftDir (0 1 0);
         dragDir (1 0 0);
         pitchAxis (0 0 0);
         magUInf 55.5;
         lRef 0.6;
         Aref 1;
         outputControl outputTime;
     }
);

Hope this helps!

Have a great day ahead!

Philippose

[DLC]

YES!!!!!!!!!!!!!!!!!!!!!!!!!!!!
it works fine now!
thanks a lot!!!!
just wondering why the same lines worked fine on the interFoam solver...

Thanks again!

DL

[surajk.garad101]

hi,


I have clearly mentioned and tried both but it didn't work for me. I am having openfoam 2112.

rhoName rhoInf;
rho rhoInf;
rhoInf 1.0;