
[Sponsors] 
July 10, 2013, 08:24 

#21 
New Member
reza sadeghi
Join Date: May 2013
Posts: 16
Rep Power: 9 
Hi.
I'am going to simulate a flow around NACA0009 at 5 degree AOA. I used simpleFoam solver and my setup is same as the airfoil2D tutorial. when i get the result, the forces and forceCoeffs are too less than I expected. the ratio of the forces compare with Fluent results are 1:25. I know this is weird. and I guess I did something wrong. I have done the case using Fluent and the results were good. Please give me some hints. Thanks 

July 22, 2013, 17:28 

#22 
New Member
Rafael Coelho
Join Date: Jun 2012
Location: Portsmouth
Posts: 23
Rep Power: 10 
I just reinstalled Openfoam and will run the airfoil case as a benchmark. Will post some results late this week.


July 28, 2013, 04:33 

#23 
New Member
Rafael Coelho
Join Date: Jun 2012
Location: Portsmouth
Posts: 23
Rep Power: 10 
I just ran the airFoil2D case and I got the following results:
forceCoeffs output: Cm = 15.2719 Cd = 0.231827 Cl = 1.85603 Cl(f) = 14.3439 Cl(r) = 16.2 After 350 interactions. 

July 28, 2013, 04:52 

#24 
New Member
Rafael Coelho
Join Date: Jun 2012
Location: Portsmouth
Posts: 23
Rep Power: 10 
Changing the liftDir and dragDir as suggested by tcarrigan:
functions { forces { type forceCoeffs; functionObjectLibs ( "libforces.so" ); outputControl timeStep; outputInterval 1; patches ( wall ); pName p; UName U; rhoName rhoInf; log true; rhoInf 1.225; liftDir (0.139173 0.990268 0); dragDir (0.990268 0.139173 0); pitchAxis (0 0 1); magUInf 26; lRef 1; Aref 1; } } I got the following Cl and Cd: forceCoeffs output: Cm = 15.2719 Cd = 0.0287385 Cl = 1.87023 Cl(f) = 14.3368 Cl(r) = 16.2071 My question now is: How did you (tcarrigan) get those values for liftDir and dragDir????? 

October 14, 2013, 03:46 
hi all

#25 
New Member
Baek, Donghae
Join Date: Jan 2013
Location: Seoul
Posts: 24
Rep Power: 9 
hi all
I am also facing to same problem. my case is 2d wind flow around bridge deck. experimental data is Cd = 0.245 Cl = 0.028 but my openfoam results were calculated as 0.002, 0.001... the order of coefficients is quite different to experimental data. so I did it myself using pressure field. I extracted pressure value from paraview after slicing mesh to obtain 2d value. then, I got Force components,generating Normal component of surface and integrating. this values are almost similar to experimental data Cd : 0.224 Cl : 0.001 but to do this, I should waste my time and large storage since Values should be 1000Hz. I dont know why openfoam output is wrong. my code is same to yours. functions { forces { type forces; functionObjectLibs ( "libforces.so" ); // lib to load outputControl timeStep; outputInterval 1; patches ( bridge ); // change to your patch name // name of fields pName p; UName U; log true; // dump to file rhoName rhoInf; rhoInf 1.25; CofR ( 2.3 0.7569 0 ); log on; } forcesCoeffs { type forceCoeffs; functionObjectLibs ( "libforces.so" ); outputControl timeStep; outputInterval 1; patches ( bridge ); pName p; UName U; log true; rhoName rhoInf; rhoInf 1.25; CofR ( 2.3 0.7569 0 ); liftDir ( 0 1 0 ); dragDir ( 1 0 0 ); pitchAxis ( 0 0 1 ); magUInf 10; lRef 0.353; Aref 0.353; } } If you guys solved this problem, please help me 

October 14, 2013, 04:10 

#26 
New Member
Rafael Coelho
Join Date: Jun 2012
Location: Portsmouth
Posts: 23
Rep Power: 10 
Check your liftdir and dragdir axis. It depends on your geometry.


October 14, 2013, 05:50 
thanks

#27  
New Member
Baek, Donghae
Join Date: Jan 2013
Location: Seoul
Posts: 24
Rep Power: 9 
Quote:
thank you for reply in my case, inlet is left side, outlet is right side and top and bottom is wall, of course, front and back is empty for 2d. the object is a deck of bridge so I think directions of drag and lift is right. I don't know what the problem is..... anyway thank you for your reply 

October 14, 2013, 14:51 

#28 
New Member
reza sadeghi
Join Date: May 2013
Posts: 16
Rep Power: 9 
Hi Baek
with using checkMesh check the depth of your geometry. using with fluent in 2d cases the depth be considered a unite. while in OF cases it depends on the depth of your 3d geometry . so the length of the cell in z direction will affect the reference values. good luck! 

October 17, 2013, 08:03 
Thanks

#29  
New Member
Baek, Donghae
Join Date: Jan 2013
Location: Seoul
Posts: 24
Rep Power: 9 
Quote:
Thank you for your advise. I think that this problem is almost sloved. my case is 2D on xy plane and z direction has 0.01 length. (5x1.5x0.01) first, I divided force by z length(0.01). after that, I calculated Cd,Cl directly using F/(1/2)*rho*U^2*L finally I got Cd : 0.29 Cl : 0.1853 observation data in experiment is Cd: 0.21 Cl: 0.028 Cd is almost similar to observation data but Cl is quite differnt. I guess that the reason why Cl is quite diffent is due to geometry. My geometry was simplified quite much. Thank you for your advise and I appreciate for Rafael_Coelho's advise 

March 18, 2016, 08:01 

#30  
Senior Member
Join Date: Mar 2016
Posts: 133
Rep Power: 6 
Quote:
Sorry but for airfoil2D example I have U (25.75 3.62 0) and therfore an angle of attack of 8°. So, i have liftdir (sin8 cos8 0) but because the direction of drag is the opposite of flux i think that dragdir (cos8 sin8 0). What do you think about? 

March 18, 2016, 08:04 

#31  
Senior Member
Join Date: Mar 2016
Posts: 133
Rep Power: 6 
Quote:


March 11, 2017, 21:56 

#32  
Member
Mehdi Mortazawy
Join Date: Mar 2017
Posts: 30
Rep Power: 5 
Quote:
That is not true. If you refer to the famous textbook of Fundamentals of Aerodynamics by Anderson, in chapter 1 you will see that LiftDir: [sin(a) cos(a) 0] DragDir: [cos(a) sin(a) 0] Also, I agree with Reza, in OpenFOAM it does matter the depth in zdirection(unlike in Fluent), as the forces are essentially divided by lRef. For the Airfoil2D case I get the following results for cm, cd, cl respectively: iter:350 Cm:1.528235e+01 CD:2.858215e02 CL:1.871433e+00 

Tags 
airfoil2d, forcecoefficient, simplefoam 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Trying to run a benchmark case with simpleFoam  spsb  OpenFOAM  3  February 24, 2012 09:07 
SimpleFOAM + SSTModel + problem with convergence  A.Devesa  OpenFOAM Running, Solving & CFD  0  November 9, 2010 04:43 
Can I solve this problem by Fluent?  Kai_kc  FLUENT  1  October 27, 2010 05:29 
natural convection problem for a CHT problem  SeHee  CFX  2  June 10, 2007 06:29 
Adiabatic and Rotating wall (Convection problem)  ParodDav  CFX  5  April 29, 2007 19:13 