
[Sponsors] 
March 23, 2010, 12:41 
kw turbulent model on a blade section

#1 
Senior Member
Join Date: Feb 2010
Posts: 213
Rep Power: 8 
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 kw 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. Last edited by vaina74; March 25, 2010 at 06:19. 

March 25, 2010, 04:17 

#2 
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 13 
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: http://www.cfdonline.com/Forums/ope...esv16a.html Enjoy. Mad 

March 25, 2010, 06:15 

#3 
Senior Member
Join Date: Feb 2010
Posts: 213
Rep Power: 8 
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 komega 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 enjoy? I'm getting mad! 

March 25, 2010, 07:15 

#4 
New Member
Join Date: Feb 2010
Posts: 24
Rep Power: 7 
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 (?)) 

March 25, 2010, 12:31 

#5 
Senior Member
Join Date: Feb 2010
Posts: 213
Rep Power: 8 
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. 

March 25, 2010, 17:19 

#6  
Senior Member
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 13 
Hello Vaina...
Quote:
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. 

March 26, 2010, 09:02 

#7 
Senior Member
Join Date: Feb 2010
Posts: 213
Rep Power: 8 
Thanks you, Maddalena. I split this long thread and move it: turbulence at boundaries and forces evaluating.


March 27, 2010, 09:25 

#8 
Senior Member
Sandy Lee
Join Date: Mar 2009
Posts: 207
Rep Power: 9 
Opps, I almost forget the force. I ever heard of that many people said it was difficult to get correct them ....


Thread Tools  
Display Modes  


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  alayyubi  Main CFD Forum  3  February 18, 2007 08:20 
turbulent model for diaphragm: wall funct, Y/Y*,..  JeanMichel M.  FLUENT  0  March 5, 2001 12:03 