
[Sponsors] 
June 4, 2012, 20:33 
Problem in simpleFoam airFoil2D forceCoeffs

#1 
New Member
venkat
Join Date: Apr 2012
Posts: 10
Rep Power: 7 
Hey guys,
I'm new to OpenFOAM and I started out with trying to run the preexisting airFoil2D case using simpleFoam. I've also added the necessary changes to my controlDict to print out the force coefficients but I've not changed any of the control variables from their default values. The output after 341 iterations is as follows, SIMPLE solution converged in 341 iterations forceCoeffs output: Cd = 0.231573 Cl = 1.85513 Cm = 15.2647 Cl(f) = 16.1922 Cl(r) = 14.3371 End The coeffs have converged as per plots of forceCoeffs, but is of wrong value My controlDict (which I'm not able to upload for some reason) is, FoamFile { version 2.0; format ascii; class dictionary; location "system"; object controlDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // application simpleFoam; startFrom startTime; startTime 0; stopAt endTime; endTime 500; deltaT 1; writeControl timeStep; writeInterval 50; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression off; timeFormat general; timePrecision 6; runTimeModifiable true; functions { forces { type forceCoeffs; functionObjectLibs ( "libforces.so" ); outputControl timeStep; outputInterval 1; patches ( wall ); pName p; UName U; rhoName rhoInf; // Indicates incompressible log true; rhoInf 1; // Redundant for incompressible liftDir (0 1 0); dragDir (1 0 0); // CofR (0 0 0); // Axle midpoint on ground pitchAxis (0 0 1); magUInf 26; lRef 1; // Wheelbase length Aref 1; // Estimated } } // ************************************************** *********************** // I'll be really grateful if someone could help me out. Thanks, venkat 

June 6, 2012, 17:04 

#2 
Member
Elh. A2. BAH
Join Date: Jan 2012
Posts: 64
Rep Power: 7 
I did run this case and obtain almost the same results.
I also did it the forces instead of the forceCoefs. and the drag was still negative. It would be great if someone has some expertise on this matter. Best regards. 

June 6, 2012, 19:13 

#3 
Senior Member

First of all, I'm not sure whether 341 iterations are enough.
Secondly, you should average the forces among 500 iterations or something, not just look at a single iteration values. 

June 7, 2012, 05:08 

#4 
Member
The True
Join Date: Dec 2010
Posts: 80
Rep Power: 8 
lref and Aref are unknown, so you should not try to get the right coefficients.
If the simulation (p, velocity) goes well than it is oke. 

June 11, 2012, 18:47 
Persisting problems

#5 
New Member
venkat
Join Date: Apr 2012
Posts: 10
Rep Power: 7 
Thank you lovecraft22 and eren10 for your replies.
But my problems are apparently more deep rooted. Problem 1: The default case does not proceed any further than 341 iterations. The value of Cd = 0.231 and Cl = 1.855 are the values after convergence as well as averaging a given number of terms. The flow field looks to be right as well. The main purpose behind me trying to run the default case was to make sure the additional lines added to controlDict to get the force coefficients would also work in a different case. Problem 2: I set up a case using an Ogrid (using Pointwise) for flow over an airfoil with parameters the same as the tutorial case (26 m/s, 8 degree AoA) and ran it till 10,000 steps. I used the same controlDict as before to print out the force coefficients. Cd = 6e05 Cl = 0.00078 Is there an alternate way to get Cl and Cd or is there a glaring mistake in the way that I've set up the problem? If you could send me a case of '2D flow over airfoil' that works with OpenFOAM with good results, it would help me a lot. Please help! Thanks again, Venkat 

June 12, 2012, 06:53 

#6 
Member
The True
Join Date: Dec 2010
Posts: 80
Rep Power: 8 
First check if the residuals are decreasing for the tutorial case.
Than check for your own simulation also the residuals. Apparantly, there is something wrong in the boundary conditions. 

June 12, 2012, 07:46 

#7 
New Member
Gregor Seljak
Join Date: Oct 2010
Posts: 21
Rep Power: 9 
What is your angle of attack? If it is not 0, you need to change liftDir and dragDir in controlDict file. Direction of liftDir must be perpendicular to airflow direction and dragDir must point in opposite direction than airflow.


June 13, 2012, 11:59 
Change in controlDict

#8  
New Member
venkat
Join Date: Apr 2012
Posts: 10
Rep Power: 7 
Quote:
liftDir ( sin(alpha) cos(alpha) 0); dragDir ( cos(alpha) sin(alpha) 0); I tried running it with this, but the results didn't change much. Also, for the tutorial case, the residuals dropped to low levels. So the problem is only in the way that the force coefficient values get printed out Thanks, Venkat 

July 8, 2012, 16:08 

#9 
New Member
Rafael Coelho
Join Date: Jun 2012
Location: Portsmouth
Posts: 23
Rep Power: 7 
I am facing the same problem. Any news of how to get the right Cl Cd?


July 12, 2012, 01:22 
Suggestion

#10 
New Member
venkat
Join Date: Apr 2012
Posts: 10
Rep Power: 7 
Hey Rafael,
A suggestion would be to plot the Cp along x/c and integrate. 

July 12, 2012, 09:50 

#11  
Senior Member
Travis Carrigan
Join Date: Jul 2010
Location: Arlington, TX
Posts: 147
Rep Power: 9 
Quote:
For the airfoil2D example I get the following results: Cd = 0.0288648 Cl = 1.86931 

July 12, 2012, 15:42 

#12 
New Member
Rafael Coelho
Join Date: Jun 2012
Location: Portsmouth
Posts: 23
Rep Power: 7 
junkie71189 thanks for your reply. I think the force is given for the whole surface, so the Cd and Cl are already integrated, right?
tcarrigan, How are you getting these values? Could you please please your controlDict? Thank you! 

July 12, 2012, 15:58 

#13  
New Member
venkat
Join Date: Apr 2012
Posts: 10
Rep Power: 7 
Quote:
tcarrigan, thank you for your correction. Can you shed some light on the lref and Aref used for the default case? 

July 12, 2012, 16:33 

#14 
Senior Member
Travis Carrigan
Join Date: Jul 2010
Location: Arlington, TX
Posts: 147
Rep Power: 9 
lRef is a reference length and Aref is a reference area. These values are used to compute the coefficients of lift, drag, and pitching moment. Because this is a 2D case and the airfoil has a unit length, therefore, lRef=1 and Aref=1. If this were a 3D calculation, lRef would be something like the mean chord length and Aref could be wing area.
To get Cl there is no need to extract Cp and sum them up for a total lift coefficient. By setting up the appropriate reference values in the forceCoeffs (like below), OpenFOAM will compute Cl for you. I believe the AOA for the airfoil2D exampel is 8deg. Here are the reference values I used: 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; } 

July 15, 2012, 07:19 

#15 
New Member
Rafael Coelho
Join Date: Jun 2012
Location: Portsmouth
Posts: 23
Rep Power: 7 
Thank you tcarrigan.
It makes sense now. I am using the same code on the wigley tutorial. But the values are very wrong. Do you know if Aref should be the total area or only the wetted (water portion) area? Besr regards, Rafael 

July 15, 2012, 16:21 

#16 
Senior Member
Travis Carrigan
Join Date: Jul 2010
Location: Arlington, TX
Posts: 147
Rep Power: 9 
For ship resistance prediction I believe you should use the wetted area, the area below the water line.


October 28, 2012, 20:17 

#17 
Member
R. P.
Join Date: Jul 2010
Posts: 72
Rep Power: 9 
Hi everyone,
I am trying to calculate the drag, lift and pitchingmoment coefficients for a flow over a probe. The code structure below works fine when the flow is perpendicular to the probe. However, when I changed the angle of attack I got a rude difference for lift and pitchingmoment when compared with experimental data (the drag values is OK). I guess, this difference is related to the vectors (liftDir (0 1 0); dragDir (1 0 0); pitchAxis (0 0 1)). I this this vectors values is just valid for a parallel flow, isn't it ? Anybody knows how to change this vectors according to a certain angle of attack ? I just need to use : liftDir ( sin(alpha) cos(alpha) 0); dragDir ( cos(alpha) sin(alpha) 0); ?? Thank you very much. Rophys forces { type forces; enabled true; functionObjectLibs ( "libforces.so" ); outputControl outputTime; patches (probe); directForceDensity true; fDName fDMean; CofR (0.02 0 0); log on; } forceCoeffs { type forceCoeffs; functionObjectLibs ("libforces.so"); patches (probe); outputControl outputTime; fDName fDMean; rhoInf 1.73e5; CofR (0.02 0 0); liftDir (0 1 0); dragDir (1 0 0); pitchAxis (0 0 1); magUInf 1503.1; lRef 0.05; Aref 9.817e4; } 

April 27, 2013, 02:34 
drag and lift calculation

#18 
New Member
dss
Join Date: Jul 2009
Posts: 25
Rep Power: 10 
Hi everyone! Hi Rafael_Coelho.
I have know you have done more work about calculation of drag and lift coeffs. I am very interested in them. I would like to ask you some questions. How to define wall function? Last edited by flyingd; May 2, 2013 at 16:28. 

May 7, 2013, 10:03 
lRef and ARef for 3 element airfoils

#19  
Senior Member
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 8 
Quote:
whould you please tell me, how does "lRef" and "ARef" define for a 3 elemet airfoil? 

May 31, 2013, 04:05 

#20  
Senior Member
saeideh mohamadi
Join Date: Aug 2012
Posts: 229
Rep Power: 8 
Quote:
would you please explain more, that how should we get the "forcCoeffs" "cd & cl" from the force.dat file that is gained after finishing the analysis? thank you very much. 

Tags 
airfoil2d, forcecoefficient, simplefoam 
Thread Tools  
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 10:07 
SimpleFOAM + SSTModel + problem with convergence  A.Devesa  OpenFOAM Running, Solving & CFD  0  November 9, 2010 05:43 
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 