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

k-w turbulent model on a blade section

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 23, 2010, 12:41
Default k-w turbulent model on a blade section
  #1
Senior Member
 
Join Date: Feb 2010
Posts: 213
Rep Power: 8
vaina74 is on a distinguished road
Well, I ran my first CFD simulation. The case concerns a blade section of an open marine propeller. The hydrofoil is about 0,3 m long, the Reynolds number is about 1.9E6. I can't believe it, the solver converges to a (I guess a wrong) solution
Now I have a few questions, I hope you have some suggestions for me.

1. The domain is large enough (see img1)?

2. I set 5 boundaries: inlet, oulet, wall (foil faces), frontAndBack and side (the rectilinear boundaries on sides). The boundary conditions are

inlet: p = zeroGradient;
U = uniform (7.30 0 0);
k = uniform 0.24;
omega = uniform 1.78

outlet: p = uniform 0;
U = zeroGradient;
k = zeroGradient;
omega = zeroGradient;

wall: p = zeroGradient;
U = uniform (0 0 0);
k = uniform 0.24; type: kqRWallFunction;
omega = uniform 1.78; type: kqRWallFunction;

side: p,U,k,omega = symmetryPlane;
frontAndBack: p,U,k,omega = empty;


are the BC right? Above all, I don't know how to specify values of the turbulence variables at the boundaries, so I set the initial k and omega as a simpleFoam tutorial case.

3. In RASProperties I set kOmegaSST RASmodel; I didn't edit the turbulenceProperties file, where SpalartAllmaras turbulentModel is set! I don't understand that, I got these settings from the simpleFoam tutorial 'motorBike', where a k-w turbulent model is applied. And what about the other coefficients (see turbulenceProperties)?

4. I didn't edit the fvSchemes and fvSolution (from the motorBike Tutorial). I don't know which are the best parameters for my case (and the solution seems to be convergent).

5. At this early stage of my work, I proposed only to do a running check of the solver simpleFoam. So in controlDict (see the attached file) i set an endTime of 10 seconds (i was curious: how much computation time?). Maybe less time is needed: which is a good final residual (see log_hydrofoil)? I guess it's better to do more and short iterations, maybe to refine the grid where I notice large gradients or to tune the parameters... Sorry, I'm a beginner

6. I obtain these results (see img2 e img3): are they realistic?

7. How can I evaluate lift and drag (CL and CD) of the hydrofoil?

Be patient, please, I'm a very beginner.
Attached Images
File Type: jpg img1.jpg (77.5 KB, 38 views)
File Type: jpg img2.jpg (13.8 KB, 35 views)
File Type: jpg img3.jpg (42.8 KB, 35 views)
Attached Files
File Type: gz files.tar.gz (5.5 KB, 9 views)

Last edited by vaina74; March 25, 2010 at 06:19.
vaina74 is offline   Reply With Quote

Old   March 25, 2010, 04:17
Default
  #2
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Hello, and welcome to the OF community!
Some observations:
1) usually domain are placed 10 chord lengths on the front and top boundary, and between 20 to 30 chord lengths on the back. If you followed this rule, your domains should be far enough.
2) BC are ok, but not the wall BC for omega: it should be omegaWallFunction and not kqRWallFunction.
5) simpleFoam is steadyState, thus the timeStep is meaningless. It counts the number of iterations, so you did not simulate 10 seconds, but 4000 iterations. And they are enough to have a converged flow.
7) Check this: Forces in V1.6
Enjoy.

Mad
maddalena is offline   Reply With Quote

Old   March 25, 2010, 06:15
Default
  #3
Senior Member
 
Join Date: Feb 2010
Posts: 213
Rep Power: 8
vaina74 is on a distinguished road
Thanks for your suggestions, Maddalena. I am still in doubt, so I go into the previous questions:

1. I can't find a shared opinion about domain extension. You suggested to me a very large one, is it suitable for an incompressible case?

2. I didn't notice the wrong omega BC, I only edited a k-omega tutorial case. I'll use omegaWallFunction. How to specify values of the turbulence variables k and omega?

3. Are correct kOmegaSST RASmodel in RASProperties and SpalartAllmaras turbulentModel?

5. The deltaT is based on the Courant number. Is the endTime linked to about 4000 iterations for a steady case? Maybe I must check the final residuals, which are the best ones in my case?

7. I already included

Code:
functions
(
forces
{
type forces;
functionObjectLibs ("libforces.so"); // Lib to load
patches (wall); // change to your patch name
rhoInf 1025; // Reference density for fluid
CofR (0 0 0); // Origin for moment calculations
}
forceCoeffs
{
type forceCoeffs;
functionObjectLibs ("libforces.so");
patches (wall); // change to your patch name
rhoInf 1025;
CofR (0 0 0);
liftDir (0 1 0);
dragDir (1 0 0);
pitchAxis (0 0 0);
magUInf 7.30;
lRef 0.305;
Aref 0.001525;
}
);
// Definition of terms:
// 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
// Definition of terms:
// 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
but I'm not sure about lRef and Aref meanings and I got some OpenFOAM errors. I'll post a new thread about that.

enjoy? I'm getting mad!
vaina74 is offline   Reply With Quote

Old   March 25, 2010, 07:15
Default
  #4
New Member
 
Join Date: Feb 2010
Posts: 24
Rep Power: 7
cboss is on a distinguished road
to 2) As I understand your question you would like to get inlet boundary conditions for k and omega.
For a first guess I would use:
k: The CFX reference points out, that if no data is available, 5% "intensity" can be used. This means, that the fluctuation velocity is 5% of your global velocity.
u_turb = 0.05 * U
k = 3/2 u_turb^2

omega: Here I would use something I'm not sure if it's correct, but should work.
omega = 1/beta_star * sqrt(k) / L
beta_star = 0.09 (from turbulence model)
L = characteristic length (I would use the chord length here (?))
cboss is offline   Reply With Quote

Old   March 25, 2010, 12:31
Default
  #5
Senior Member
 
Join Date: Feb 2010
Posts: 213
Rep Power: 8
vaina74 is on a distinguished road
For a first guess, I already evaluated an inlet turbulent energy, based on the turbulence intensity wiki page (1% for my case). I'm really in trouble with the inlet turbulence frequency: I know the model is very sensitive to the inlent freestream turbulence properties.
w=e/k and then? I'm not able to evaluate the 'best' turbulence length scale for an outer flow

Last edited by vaina74; March 25, 2010 at 12:54.
vaina74 is offline   Reply With Quote

Old   March 25, 2010, 17:19
Default
  #6
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Hello Vaina...
Quote:
I'm not sure about lRef and Aref meanings
I would use lRef = chord lenght, and Aref = 1, since your simulation is 2d.In any case, could you post the OF error message you have?
As for the k and omega value, I suggest you to check in Fluent user guide for some advices.
Bye,
mad

Last edited by maddalena; March 26, 2010 at 03:13.
maddalena is offline   Reply With Quote

Old   March 26, 2010, 09:02
Default
  #7
Senior Member
 
Join Date: Feb 2010
Posts: 213
Rep Power: 8
vaina74 is on a distinguished road
Thanks you, Maddalena. I split this long thread and move it: turbulence at boundaries and forces evaluating.
vaina74 is offline   Reply With Quote

Old   March 27, 2010, 09:25
Default
  #8
Senior Member
 
Sandy Lee
Join Date: Mar 2009
Posts: 207
Rep Power: 9
sandy is on a distinguished road
Opps, I almost forget the force. I ever heard of that many people said it was difficult to get correct them ....
sandy 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
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36
Half laminar and turbulent model trying to solve Andrew Clarke FLUENT 5 May 19, 2008 13:40
turbulent model jack FLUENT 1 September 17, 2007 04:22
Similarity on helicopter blade model al-ayyubi Main CFD Forum 3 February 18, 2007 08:20
turbulent model for diaphragm: wall funct, Y/Y*,.. Jean-Michel M. FLUENT 0 March 5, 2001 12:03


All times are GMT -4. The time now is 09:47.