[mihaipruna]

The same dictionary worked in previous versions.
The case solves and there should be a net force because pressure integration shows a number greater than 0.
Here is the forceCoeffs dictionary:

forces

{

    type        forceCoeffs;

    functionObjectLibs ( "libforces.so" );

    outputControl timeStep;

    outputInterval 1;

    patches     (

        "vol1face1"

        "vol1face2"

        "vol1face3"

        "vol1face4"

        "vol1face5"

        "vol1face6"

    );

    pName       p;

    UName       U;

    rhoName     rhoInf;      // Indicates incompressible

    log         true;

    rhoInf      1;           // Redundant for incompressible

    liftDir     (-0.000000 1.000000 0.000000);

    dragDir     (1.000000 0.000000 0.000000);

    CofR        (0.72 0 0);  // Axle midpoint on ground

    pitchAxis   (0 0 1);

    magUInf       100.0000;

    lRef            1.0000;

    Aref            6.0000;

    }

[wyldckat]

Hi Mihai,

I haven't tested this, but comparing the tutorial "tutorials/incompressible/simpleFoam/motorBike" between versions:

• OpenFOAM 2.1.x: https://github.com/OpenFOAM/OpenFOAM...em/forceCoeffs
• OpenFOAM 2.2.x: https://github.com/OpenFOAM/OpenFOAM...em/forceCoeffs

You'll see that there is a new entry:

binData
    {
        nBin        20;          // output data into 20 bins
        direction   (1 0 0);     // bin direction
        format      gnuplot;
        cumulative  yes;
    }

In theory, you should have seen in your solver log folder a message indicating the missing entry "binData".


Best regards,
Bruno

[mihaipruna]

Bruno
I tried to add that part and got an error.

[wyldckat]

Hi Mihai,

Now I'm confused... I've ran just now the same "motorBike" case from 2.1.x, but on 2.2.0 and 2.2.x and it calculated the forces... although I haven't compared the results...

But one thing I noticed in the file "log.simpleFoam" is that it made a lot of complaints about the div schemes:

--> FOAM Warning : 
    From function gaussConvectionScheme
    in file finiteVolume/convectionSchemes/gaussConvectionScheme/gaussConvectionScheme.H at line 123
    Reading "/home/bmss/OpenFOAM/bmss-2.1.x/run/tutorials/incompressible/simpleFoam/motorBike/system/fvSchemes.divSchemes.div(phi,U)" at line 30
    Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.
    To remove this warning switch off 'boundedGauss' in "/home/bmss/OpenFOAM/OpenFOAM-2.2.x/etc/controlDict"
smoothSolver:  Solving for Ux, Initial residual = 0.226116, Final residual = 0.0133515, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.275451, Final residual = 0.0161505, No Iterations 3
smoothSolver:  Solving for Uz, Initial residual = 0.172255, Final residual = 0.0161645, No Iterations 2
GAMG:  Solving for p, Initial residual = 0.106832, Final residual = 0.00781284, No Iterations 2
time step continuity errors : sum local = 0.0152865, global = 0.00268025, cumulative = 0.00268025
--> FOAM Warning : 
    From function gaussConvectionScheme
    in file finiteVolume/convectionSchemes/gaussConvectionScheme/gaussConvectionScheme.H at line 123
    Reading "/home/bmss/OpenFOAM/bmss-2.1.x/run/tutorials/incompressible/simpleFoam/motorBike/system/fvSchemes.divSchemes.div(phi,omega)" at line 32
    Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.
    To remove this warning switch off 'boundedGauss' in "/home/bmss/OpenFOAM/OpenFOAM-2.2.x/etc/controlDict"
smoothSolver:  Solving for omega, Initial residual = 0.00480145, Final residual = 0.000399432, No Iterations 3
--> FOAM Warning : 
    From function gaussConvectionScheme
    in file finiteVolume/convectionSchemes/gaussConvectionScheme/gaussConvectionScheme.H at line 123
    Reading "/home/bmss/OpenFOAM/bmss-2.1.x/run/tutorials/incompressible/simpleFoam/motorBike/system/fvSchemes.divSchemes.div(phi,k)" at line 31
    Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.
    To remove this warning switch off 'boundedGauss' in "/home/bmss/OpenFOAM/OpenFOAM-2.2.x/etc/controlDict"
smoothSolver:  Solving for k, Initial residual = 1, Final residual = 0.0477205, No Iterations 3
ExecutionTime = 12.15 s  ClockTime = 12 s

Are you getting these same messages?

And what was the error you got when you used the "binData" entry?

Best regards,
Bruno

[dkokron]

Bruno,

I got those same warnings when I converted from 2.1.x to 2.2.x. They are just informational. The numerics didn't change when I re-ran my case with the now recommended 'bounded' schemes. See http://www.openfoam.org/version2.2.0/numerics.php for the details.

Dan

[hakonbar]

I had the same problem when I upgraded from 2.1 to 2.2. Apparently a bug was introduced in the latest update so that if you record the forces on several surfaces, only those on the last surface in your list will be written to file.

If you define the body on which you wish to measure the forces as a single surface, it'll probably work, but the bug has been fixed in the latest git release.

Read this thread for more info:
http://www.cfd-online.com/Forums/ope...s-airfoil.html

[harsha_kulkarni]

Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.

when I use bounded Gauss it produce following error floating point error

with unbound 'Gauss' it not produce any error

[sibo]

Hi guys,

how did you solve this problem? I run into the same problem here.

Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.

Although there are many warnings, there is no error. Can we ignore this warning?
I am using the OpenFOAM-3.0.1

Thanks a lot!

[Andela]

Hi Sibo,

I am also using OF 3.0.1., and I got same wqarnings.
After adding in fvSchemes:
div(phi,T) bounded Gauss upwind;
the warnings dissapeared, and the simulation runs without any errors.

[sibo]

Thanks for your reply!!