[terrybarnaby]

Hi, I have updated from 1.5 to 1.6 (GIT source). I have modified some of my cases control files to get OpenFOAM 1.6 to work but I am having problems with forces in simpleFoam.
I get the error message:
--> 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.
My controlDict force configuration is:

functions
(
forces
{
type forces;
functionObjectLibs ("libforces.so");
outputControl outputTime;

// Patches to sample
patches (car_car);
// Name of fields
pName p;
Uname U;
// Dump to file
log true;
// Density
rhoInf 1.17;
// Centre of rotation
CofR (0 0 0);
}

forceCoeffs
{
type forceCoeffs;
functionObjectLibs ("libforces.so");
outputControl outputTime;

// Patches to sample
patches (car_car);
// Name of fields
pName p;
Uname U;
// Dump to file
log true;
// Density
rhoInf 1.17;
// Centre of rotation
CofR (0 0 0);

// Direction for lift
liftDir (0.0 1.0 0.0);
// Direction for drag
dragDir (1.0 0.0 0.0);

// Pitching axis
pitchAxis (0 0 0);

magUInf 13.0;

lRef 2.5;
Aref 0.296256;
}
);

Any one have any idea what is wrong ?

[terrybarnaby]

Looking at the source code it looks like I need to add: "rhoName rhoInf;" to the "forces" and "forceCoeffs" entreis in controlDict or provide a "rho" initial conditions file in "0".
This appears to work ...

[MadsR]

Nice find, it worked for me too.

/Mads

[ronaldo]

could someone tell me the best way to simulate the Flow over a Cylinder?
Laminare, k-epsilon and k-omega!

[openfoam_user]

Terry,

I am using MRFSimpleFoam - OpenFoam-1.6.x.

I get the following message error :

Starting time loop

--> FOAM Warning :
From function void forces::read(const dictionary& dict)
in file forces/forces.C at line 278
Could not find U, p or rho in database.
De-activating forces.

My controlDict is :

functions
(
forces
{
type forces;
functionObjectLibs ("libforces.so"); //Lib to load
patches (object1); // change to your patch name
pName p;
Uname U;
rhoName rho;
rhoInf 1.225; //Reference density for fluid
CofR (0 0 0); //Origin for moment calculations
outputControl timeStep;
outputInterval 1;
}
);

How do I modify my controlDict file ?

Regards,

Stephane

[terrybarnaby]

Hi,

You need to add:

rhoName rhoInf;
rhoInf 1.17;

instead of:

rhoName rho;
rhoInf 1.225; //Reference density for fluid

I think...

Cheers


Terry

[terrybarnaby]

Obviously rhoInf should be set how you need it

[openfoam_user]

Thanks Terry,

Now it works fine !

One more question.
And if I want to have the forces results like below (tail -f log) in the log file ?

Courant Number mean: 0.000625962 max: 0.0181186
DILUPBiCG: Solving for Ux, Initial residual = 8.58271e-05, Final residual = 5.68736e-12, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.000135717, Final residual = 1.58931e-11, No Iterations 1
DICPCG: Solving for p, Initial residual = 0.000308555, Final residual = 2.98446e-06, No Iterations 6
DICPCG: Solving for p, Initial residual = 5.6599e-06, Final residual = 9.87842e-07, No Iterations 193
DICPCG: Solving for p, Initial residual = 1.97131e-06, Final residual = 8.93472e-07, No Iterations 1
DICPCG: Solving for p, Initial residual = 9.0792e-07, Final residual = 9.0792e-07, No Iterations 0
time step continuity errors : sum local = 9.67148e-15, global = -1.15687e-16, cumulative = -1.07021e-10
DICPCG: Solving for p, Initial residual = 9.19959e-07, Final residual = 9.19959e-07, No Iterations 0
DICPCG: Solving for p, Initial residual = 9.19959e-07, Final residual = 9.19959e-07, No Iterations 0
DICPCG: Solving for p, Initial residual = 9.19959e-07, Final residual = 9.19959e-07, No Iterations 0
DICPCG: Solving for p, Initial residual = 9.19959e-07, Final residual = 9.19959e-07, No Iterations 0
time step continuity errors : sum local = 9.79972e-15, global = -1.14472e-16, cumulative = -1.07021e-10
ExecutionTime = 25809.3 s ClockTime = 77462 s
forces output:
forces(pressure, viscous)((3.36459 -0.00234243 9.49148e-20) (0.365777 -2.56403e-05 -1.76832e-22))
moment(pressure, viscous)((3.41853e-19 -8.54044e-18 -0.00215479) (-8.87561e-22 1.48373e-20
0.0157578))
forceCoeffs output:
Cd = 152.26
Cl = -0.0966561
Cm = -1.91544e-17
Time = 2.417


Stephane.

[terrybarnaby]

Sorry, I am only a novice at this so I don't know how to do that.

You could try adding:
log true;

I'm not sure what that does ...

[griztown]

Hi,

Is there not a website or tutorial anywhere that gives some instructions for using the forces function? Does it really take digging through the source code? Any links or tips would be much appreciated!

Thanks

[AirS]

Hi all,

I want to investigate the forces acting on a cylinder so I use the entry "forces" in the controlDict,
It works well but in the file .dat I've got something like that:

forces(pressure, viscous)((3.36459 -0.00234243 9.49148e-20) (0.365777 -2.56403e-05 -1.76832e-22))
moment(pressure, viscous)((3.41853e-19 -8.54044e-18 -0.00215479) (-8.87561e-22 1.48373e-20))

What does (pressure, viscous) mean ? I want to compute all the forces that is to say Fx,Fy,Fz.
I can't see them anywhere in the data file...
Is there something I'm missing?
Thanks.

[terrybarnaby]

As far as I know:
Pressure force is the force on the object due directly to pressure differences.
Viscous force is the force due to the "friction" of the fluid passing over the objects surface.

To get the total force acting on the object you need to add the pressure components to the viscous components.

[g.redondo]

Hi all,

I was trying to include the density in the forces.C file and I found that there are already some lines regarding to it. Therefore I wonder if multi-phase is already supported in OF1.6.

If so, how should the controlDict entry be. If it doesn't support it, how should it be included? The most important line would be the following. I think it should be:

vectorField vf = (Sfb[patchi] & devRhoReffb[patchi])*rho.boundaryField()[patchi];

and it is:

vectorField vf = Sfb[patchi] & devRhoReffb[patchi]

has anyone fixed this?

Gonzalo

[jploz]

Hi Gonzalo,

no, the forces object supplied with OF 1.6 does not support multiphase flow. It uses the prescribed density "rhoInf" when calculating the viscous forces (as I already wrote here http://www.cfd-online.com/Forums/ope...ip-flow-2.html) which is obviously not correct in the case of compressible flow and flow involving more than a single incompressible phase. If you would use a constant density in such case your resulting viscous forces would differ a lot.

In order to fix this, you need to read the current density field and use that instead of the defined "rhoInf".

Good luck.
Jean-Peer

[83_Ale_83]

Originally Posted by griztown

Hi,

Is there not a website or tutorial anywhere that gives some instructions for using the forces function? Does it really take digging through the source code? Any links or tips would be much appreciated!

Thanks

Quote,
anyone can help me? I'am trying to calculate the drag and lift on a cylinder with simplefoam..any advise?

Thank you

[santos]

Hi,

Put something like this in your system/controlDict, changing accordingly to your situation:

functions
{
forces
{
type forces;
functionObjectLibs ("libforces.so"); //Lib to load
patches (sphere_region0); // change to your patch name
rhoName rhoInf;
rhoInf 1000; //Reference density for fluid
CofR (2 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 (sphere_region0);
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;
}

}

Regards,
Jose Santos

[83_Ale_83]

Impressive

I have put in my controlDict file this code:

type forces;
functionObjectLibs ("libforces.so"); //Lib to load
patches (cilindro); // change to your patch name
pName p;
Uname U;
rhoName rhoInf;
rhoInf 1.17;
CofR (0 0 0); //Origin for moment calculations
outputControl timeStep;
outputInterval 1;

"My" code calculates the forces, your code calculates the coefficient right?
With regards

[santos]

"My" code calculates both the forces and their coefficients ;-)

[83_Ale_83]

Originally Posted by santos

"My" code calculates both the forces and their coefficients ;-)

Thank you, I tried and it works very well

[83_Ale_83]

Hello to everybody,
I'm trying to remove the brackets and the header from forces.dat output file, any advise please?

Thank you in advance