CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

Cl(f) and Cl(r) what it means?

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   June 13, 2013, 08:35
Default Cl(f) and Cl(r) what it means?
  #1
hhh
Senior Member
 
kumar
Join Date: Nov 2011
Posts: 115
Rep Power: 5
hhh is on a distinguished road
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

Last edited by wyldckat; June 15, 2013 at 15:17. Reason: Added the [CODE] delimiters
hhh is offline   Reply With Quote

Old   June 15, 2013, 15:34
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,258
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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
wyldckat is offline   Reply With Quote

Old   June 16, 2013, 05:32
Default
  #3
hhh
Senior Member
 
kumar
Join Date: Nov 2011
Posts: 115
Rep Power: 5
hhh is on a distinguished road
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


hhh is offline   Reply With Quote

Old   June 16, 2013, 08:55
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,258
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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
wyldckat is offline   Reply With Quote

Old   June 17, 2013, 03:08
Default
  #5
hhh
Senior Member
 
kumar
Join Date: Nov 2011
Posts: 115
Rep Power: 5
hhh is on a distinguished road
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.
hhh is offline   Reply With Quote

Old   June 17, 2013, 17:04
Default
  #6
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,258
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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
wyldckat is offline   Reply With Quote

Old   June 18, 2013, 02:46
Default
  #7
hhh
Senior Member
 
kumar
Join Date: Nov 2011
Posts: 115
Rep Power: 5
hhh is on a distinguished road
Thanks Bruno, Have a nice Day
hhh is offline   Reply With Quote

Old   June 18, 2013, 05:55
Default
  #8
hhh
Senior Member
 
kumar
Join Date: Nov 2011
Posts: 115
Rep Power: 5
hhh is on a distinguished road
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
Attached Images
File Type: jpg Image 1.jpg (17.2 KB, 33 views)
File Type: jpg Image2.jpg (19.9 KB, 27 views)

Last edited by hhh; June 18, 2013 at 10:48.
hhh is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Failed 1 mesh check camoesas OpenFOAM 24 September 18, 2013 03:42
kEpsilon divergence s.m OpenFOAM Running, Solving & CFD 0 May 27, 2013 09:30


All times are GMT -4. The time now is 18:42.