CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)
-   -   Cl(f) and Cl(r) what it means? (https://www.cfd-online.com/Forums/openfoam/119279-cl-f-cl-r-what-means.html)

hhh June 13, 2013 08:35

Cl(f) and Cl(r) what it means?
 
hai friends,

I am doing 2d airfoil analysis, i have doubt about the result i got ie Cl(f) and Cl(r) it means what? and also i mention in red colour

Code:

/*---------------------------------------------------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  2.1.0                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
Build  : 2.1.0-0bc225064152
Exec  : simpleFoam
Date  : Jun 11 2013
Time  : 14:42:35
Host  : "ubuntu"
Case  : /home/toshiba/OpenFOAM/toshiba-2.1.0/run/tutorials/incompressible/simpleFoam/ku/airFoil2D
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model SpalartAllmaras
SpalartAllmarasCoeffs
{
    sigmaNut        0.66666;
    kappa          0.41;
    Cb1            0.1355;
    Cb2            0.622;
    Cw2            0.3;
    Cw3            2;
    Cv1            7.1;
    Cv2            5;
}

No field sources present

SIMPLE: convergence criteria
field p    tolerance 1e-05
    field U    tolerance 1e-05
    field nuTilda    tolerance 1e-05


Starting time loop

Time = 1

smoothSolver:  Solving for Ux, Initial residual = 0.999993, Final residual = 0.0558381, No Iterations 4
smoothSolver:  Solving for Uy, Initial residual = 1, Final residual = 0.0760732, No Iterations 2
GAMG:  Solving for p, Initial residual = 1, Final residual = 0.0991895, No Iterations 39
time step continuity errors : sum local = 0.00119979, global = 6.26709e-16, cumulative = 6.26709e-16
smoothSolver:  Solving for nuTilda, Initial residual = 0.999999, Final residual = 0.0701398, No Iterations 4
ExecutionTime = 36.7 s  ClockTime = 37 s

forces output:
    forces(pressure,viscous)((257697 5.20299e+06 7.66604e-16),(6.53254 1.33905 -1.89121e-21))
    moment(pressure,viscous)((-3.39084e-17 -1.06156e-16 2.50963e+06),(4.47879e-23 -2.14236e-22 0.66735))

forceCoeffs output:
    Cm    = 901.996
    Cd    = 415.85
    Cl    = 1857.68
    Cl(f) = 1830.84
    Cl(r) = 26.8427


Time = 2

smoothSolver:  Solving for Ux, Initial residual = 0.623192, Final residual = 0.0517858, No Iterations 4
smoothSolver:  Solving for Uy, Initial residual = 0.445407, Final residual = 0.0284221, No Iterations 4
GAMG:  Solving for p, Initial residual = 0.711508, Final residual = 0.0608906, No Iterations 11
time step continuity errors : sum local = 0.000802196, global = 1.48748e-15, cumulative = 2.11418e-15
smoothSolver:  Solving for nuTilda, Initial residual = 0.258696, Final residual = 0.0187245, No Iterations 4
ExecutionTime = 45.88 s  ClockTime = 46 s

forces output:
    forces(pressure,viscous)((168327 3.88357e+06 2.72499e-16),(23.6262 2.65695 -2.24632e-21))
    moment(pressure,viscous)((-2.10668e-17 -5.5126e-17 1.89813e+06),(5.34685e-23 -6.75307e-22 1.37948))

forceCoeffs output:
    Cm    = 682.213
    Cd    = 301.9
    Cl    = 1385.1
    Cl(f) = 1374.76
    Cl(r) = 10.3358

please guide me

wyldckat June 15, 2013 15:34

Hi Kumar,

Most of these you can find out about them by using Google. For example, use the following text in Google:
Code:

openfoam "fileModificationChecking"
Some of the more complicated ones to find, I'll try to explain:
  • "nProcs : 1" - indicates the number of cooperative processes being used for this case. Only when used in parallel, will you see this value increase.
  • Code:

    forceCoeffs output:
        Cm    = 682.213
        Cd    = 301.9
        Cl    = 1385.1
        Cl(f) = 1374.76
        Cl(r) = 10.3358

    These are calculated because in "system/controlDict" you are using the "forceCoeffs" function object. If you look at the file given by the following command:
    Code:

    echo $FOAM_SRC/postProcessing/functionObjects/forces/forceCoeffs/forceCoeffs.C
    Or look at the one available online: https://github.com/OpenFOAM/OpenFOAM.../forceCoeffs.C
    You'll see the following code:
    Code:

                coeffs[0] = (totForce & liftDir_)/(Aref_*pDyn);
                coeffs[1] = (totForce & dragDir_)/(Aref_*pDyn);
                coeffs[2] = (totMoment & pitchAxis_)/(Aref_*lRef_*pDyn);

                scalar Cl = sum(coeffs[0]);
                scalar Cd = sum(coeffs[1]);
                scalar Cm = sum(coeffs[2]);

                scalar Clf = Cl/2.0 + Cm;
                scalar Clr = Cl/2.0 - Cm;

    Which should be somewhat self-explanatory...
Best regards,
Bruno

hhh June 16, 2013 05:32

Thanks Bruno for your kind response.

For laminar case

1. I remove nut & nu from O folder and i change p & U and in system folder
for i make changes in controldict according to my velocity

2.I didnt change in transport Properties in constant folder

3. RASProperties
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

RASModel SpalartAllmaras; [instead of
SpalartAllmaras i

change laminar]

turbulence on; [turbulence off]

printCoeffs on;


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



I think this is correct,if any thing i have to make changes,please let me know. my Reynolds number is 1000


once again thanks Bruno, you are coming forward to help me a lot


Thanks for your valuable time



wyldckat June 16, 2013 08:55

Hi Kumar,

It seems to be OK for running in laminar flow.

All other configurations that were meant for turbulence in "system/fvSolution" and "system/fvSchemes", won't be used either way, so there is no need to remove them from those two files.

Best regards,
Bruno

hhh June 17, 2013 03:08

Hai Bruno thanks a lot for your help, everything works fine.

I forgot to ask for turbulent case,while doing angle of attack 10. I set x velocity and y velocity in internal field in O folder for U

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];

internalField uniform (2.2946 0.4046 0);

boundaryField
{
inlet
{
type freestream;
freestreamValue uniform (2.2946 0.4046 0);
}

outlet
{
type freestream;
freestreamValue uniform (2.2946 0.4046 0);


but I took default value for nuTilda and nut ie .14 whatever in that folder.

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

dimensions [0 2 -1 0 0 0 0];

internalField uniform 0.14;


boundaryField
{
inlet
{
type freestream;
freestreamValue uniform 0.14;
}

outlet
{
type freestream;
freestreamValue uniform 0.14;
}

I think it seems unimportant nut & nuTilda.Actually what i understand is the internal field value is to set the same as the inlet value( velocity= 2.33 m/s)but Anyhow it will be overwritten after the first time step.


This is correct or wrong,please let me know.

wyldckat June 17, 2013 17:04

Hi Kumar,

Yes, if I remember correctly, "nut" and "nuTilda" are mostly calculated by the turbulence models. The set-up of the boundary conditions for those fields is almost just a formality, in the sense that they will be calculated if they are allowed to do so.

If I'm not mistaken, if you were to set one of the conditions in "nut" or "nuTilda" to zero gradient, such as this:
Code:

    inlet
    {
        type zeroGradient;
    }

It would still be zero gradient in the next step... assuming of course that the solver doesn't complain about this.
Another example is the "symmetry" type of condition, which the solver should allow, e.g.:
Code:

    symmetricWall
    {
        type symmetry;
    }

Best regards,
Bruno

PS: Have a look into the post the second link in my signature links to, because in it I explained how you can paste code ;)

hhh June 18, 2013 02:46

Thanks Bruno, Have a nice Day

hhh June 18, 2013 05:55

2 Attachment(s)
Hai, Bruno

I am trying to do 3D wing Analysis for Unsteady case.I took NACA0012 airfoil and extrude 5cm length from Back Face of Domain.let Reynolds number 1000 and velocity is 3m/s.

DOMAIN
Boundary Condition


Side 1- velocity inlet
Side 2-pressure outlet
Top,Bottom,Front Face-symmetry
Back Face & wing - Wall

I did meshing part in gambit.

I want to flap the wing up & down for [-5 to +5 Amplitude angle]. For this I want to see the lift and Drag. Somebody did in Fluent (Dynamic Mesh), the same thing I want to do in open foam, please see the link its you tube video (ie Flapping 3d wing -Pressure contours).

LINK: [ http://www.youtube.com/watch?v=RjwV8TzW6a8 ]

For domain, Please see the attached my image for your reference.If you have any idea, please give me your suggestions.


Thanks for your valuable Time


All times are GMT -4. The time now is 20:31.