
[Sponsors] 
October 29, 2007, 10:37 
Hello everybody,
I am runni

#81 
Member
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 17 
Hello everybody,
I am running some validation cases for a naca0012 at low angle of attack using simpleFoam and kepsilon turbulence model. Airfoil chord 1 m, inlet velocity 50 m/s, freestream viscosity 1.7894e5. I noticed that if I compile the liftDrag.C version from Vincent RIVOLA on Wednesday, September 19, 2007  09:36 am the results are quite good (if I multiply by density). However, I tried using liftDrag.C posted by Vincent RIVOLA on Thursday, September 20, 2007  03:47 am and I get a drag coefficient which is 4 orders of magnitude lower. I am checking these two files. I will keep you updated. Thank you, Alessandro 

October 29, 2007, 10:43 
Sorry, I see you have to pass

#82 
Member
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 17 
Sorry, I see you have to pass in Aref.
Howver comparing "Vincent RIVOLA on Wednesday, September 19, 2007  09:36 am" with "Vincent RIVOLA on Thursday, September 20, 2007  03:47 am " it seems like the values of turbulent and laminar drag coefficients get swapped. Alessandro 

October 29, 2007, 12:25 
Hello everybody,
using li

#83 
Member
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 17 
Hello everybody,
using liftDrag.C from "Vincent RIVOLA on Wednesday, September 19, 2007  09:36 am" and my airfoil at 0deg angle of attack I get: total Turbulent drag coefficient: 0.00034 total laminar drag coefficient: 0.00116 which I cannot explain. Even if I multiply my density, say 1.225, the total drag is way too low, as it should be ~~ 0.0058 from "theory of wing sections". I changed liftDrac.C as suggsted by " Rosario Russo on Monday, September 24, 2007  09:32 am" and now I get: total Turbulent drag coefficient: 0.00198 total laminar drag coefficient: 0.001161 Still way off. I will rerun my case with better schemes. Any comments? Thank you, Alessandro 

October 29, 2007, 13:43 
Ok, I give up.
Using the sa

#84 
Member
Alessandro Spadoni
Join Date: Mar 2009
Location: Atlanta, GA
Posts: 65
Rep Power: 17 
Ok, I give up.
Using the same mesh in fluent I get a drag coefficient of 0.0052 which is 10% away from the experimental value in "theory of wing sections." OpenFoam gives me 0.00314. Please help Alessandro 

October 29, 2007, 15:19 
Hi Alessandro,
I'm also int

#85 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 283
Rep Power: 18 
Hi Alessandro,
I'm also interested in your computations since, I am still not sure that the liftDrag utility is computing the drag correctly. To really compare the values from OpenFOAM and Fluent, I think it would be interesting to compare the Cp values found in fluent to the ones found in OpenFOAM. If these values are the same, the problem is coming from the liftdrag utility. Otherwise, the problem is coming from the computation. The same can be done by comparing velocity fields. Hope that helps. Regards, Vincent 

October 30, 2007, 22:45 
liftDrag area calculation for

#86 
Senior Member
Srinath Madhavan (a.k.a pUl)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 703
Rep Power: 21 
liftDrag area calculation for force computation is nontrivial. Please make sure that if you are working on a 2D case, the domain length in the third direction is reasonable. See Hrv's comment here to follow what I'm referring to > http://www.cfdonline.com/OpenFOAM_D...es/1/2726.html


April 24, 2008, 09:23 
Hi everybody,
I now manage

#87 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 283
Rep Power: 18 
Hi everybody,
I now manage to get some interesting results on Ahmed test case and on a real race car. Pressure and velocity fields look not so bad and some vortices can be observed in some particular regions. However I still have some doubts on my way to compute lift and drag coeffcients. Drag coefficient looks ok actually, for the ahmed body and for the race car as well. But the lift coefficient is far from the results I should have. By reading again this topic I see that some questions stayed without answer. Especially the doubts about the way to compute turbulent part. Could someone point out what is actually the best liftDrag tool which could be used with simpleFoam? Regards, Vincent 

April 24, 2008, 10:11 
Hi Vincent,
I ran a Ahmed bod

#88 
New Member
Mattia
Join Date: Mar 2009
Posts: 26
Rep Power: 17 
Hi Vincent,
I ran a Ahmed body case with 4M cells for half car in SimpleFoam, but the results I managed weren't so good: the pressure and velocity fields were quite different from experimental data. Can you describe what models and solvers you used, please? 

June 2, 2008, 17:18 
Hey Mattia,
which slant ang

#89 
New Member
Thomas Ceyrowsky
Join Date: Mar 2009
Location: Germany
Posts: 9
Rep Power: 17 
Hey Mattia,
which slant angle did you run? Turbulence modelling is not capable for getting the correct results with 25°. Additionally the flow around the 25°case is very instationary so simpleFoam has got some converging problems (at least in my calculations). Apart from that the 35°results with simpleFoam were pretty good, because the flow has got a stable character. I had positive experiences with the Realizablekepsilon model and the limitedLinear TVDInterpolation. Best regards, Thomas 

October 7, 2008, 15:16 
Hi all,
I have been doing s

#90 
Senior Member

Hi all,
I have been doing some Ahmed body drag and lift calculations and although I often get ok results for the drag coefficients, the lift coefficients I get are always in the range of 34.. Which is about 10 times too large. I am working in 2D with simpleFoam and RealizableKE, komegaSST, and SA models. Has anyone experienced difficulties with computing the lift? I would appreciate some pointers! Thank you, Louis 

October 8, 2008, 05:17 
From reading some articles, it

#91 
Senior Member
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 17 
From reading some articles, it seems a few people have. How are you calculating the lift coefficient?


October 8, 2008, 11:56 
Hi Adriano,
I use the force

#92 
Senior Member

Hi Adriano,
I use the forceCoefficients function included in OF 1.5. Also, I verify the results obtained from that with the patchIntegrate on pressure and I get values that correspond (viscous lift excluded) to what forceCoefficients gives. Aref= frontal projected area I assume there is something wrong in my pressure field but I find strange that drag forces are still reasonable. Have a good day, Louis 

October 8, 2008, 12:43 
What is your frontal area valu

#93 
Senior Member
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 17 
What is your frontal area value? What are your minimum values of surface pressure on the upper surface? Have you tried looking at the velocity fields and comparing it to the experimental data?


October 8, 2008, 13:49 
Aref=0.00288 (my mesh is 0.01

#94 
Senior Member

Aref=0.00288 (my mesh is 0.01 m thick); min pressure on upper surface is [1.5,2.08] (the lowest pressure is proportional to the drag coefficient I get); and my velocity fields look somewhat like the experimental data: two recirculation zones at the vertical back plane (and on the slant plane when slant angle is large enough), very thin B.L. on top surface, acceleration zone on the top leading edge.
The acceleration zone on the leading edge goes all the way to the wall of the vehicle and the velocity is >1 until it reaches the wall where it suddenly becomes 0. (Longitudinal vortices are excluded since Im in 2D). Also, another strange trend I noticed is that when drag is overestimated, the value of lift reduces (usually not enough to get appropriate results and the trend is not always respected). thanks for your help! (I am doing this project for my Master's thesis) Louis 

October 9, 2008, 03:29 
Is that your minimum pressre c

#95 
Senior Member
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 17 
Is that your minimum pressre coefficient? The velocity at the wall should be zero due to the noslip condition.
Do all your results converge ok? If so, how long do you run them for? Finally, what is the first wall spacing you are using (or y+ would be better)? Adriano 

October 9, 2008, 09:48 
the is actually the pressure

#96 
Senior Member

the [1.5,2.08] is actually the pressure "p" value (using a 0 reference pressure), so I assume it is in (Pa *m^3/kg). ( I wrote lowest upper surface pressure proportional to drag coefficient but I meant lowest upper surface pressure proportional to lift coefficient...)
I use the noslip condition (fixedValue velocity, value = uniform 0 on the vehicle wall) and still get velocity >1 on the cell/point next to the wall; also, pressure is zeroGradient on the vehicle wall. My results converge very well, except in a few rare cases. As for my y+ value, it is not consistent through the whole wall and I have a hard time getting it outsite of the "intertide" zone of 1<yplus<30. (Allthough Im not sure this is an issue with models other than SA) Here are a few Yplus values I get: min: 6.9669 max: 90.5637 average: 59.6992 (SA) min: 0.418455 max: 18.4831 average: 8.81904 (SA) min: 12.8556 max: 334.043 average: 155.761 (RKE) min: 12.0163 max: 301.83 average: 144.64 (RKE) Also, convergence is not a good (or maybe just very slow) when I try to lower my value of Yplus by refinement at the wall. min: 0.128637 max: 18.1411 average: 6.55086 (komegaSST, with pretty fine mesh) Have a good day! Louis 

October 9, 2008, 10:00 
Forgot to add...
It is my m

#97 
Senior Member

Forgot to add...
It is my minimum pressure, yes. And i run the calculation until drag is constant (at least to the 10^4), when possible; at that point there are no more iterations per "timestep" on velocities and sometimes 1 on pressure. (Thats usually 2000030000 iterations. But again, with the smaller y+ it is not as obvious to run the simulations until convergence! Also, concerning the velocity field, the velocity near the bottom leading edge of the vehicle lower than on the upper leading edge. Louis 

October 24, 2008, 19:58 
Hi Adriano,
Do you have any

#98 
Senior Member

Hi Adriano,
Do you have any hints to help me get better lift coefficients? I am currently trying to see if changing the bottom surface to a fixed one, as in the experiments, will help. So far my results still have a very high lift coefficient. regards, Louis 

October 27, 2008, 08:43 
Hi Louis,
What boundary con

#99 
Senior Member
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 17 
Hi Louis,
What boundary condition did you apply to the lower surface wall previously? If possible, would you be able to email me your mesh and I can run it myself and take a look at it? In the meantime, I'd try, if possible, to get a mesh with a y+ of between 30 (abs. min) and 300 and rerun with the ke model, and have a look at the results. It will give you a better idea before you attempt a more challenging y+=1 mesh. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
3d test case  Hassan Raiesi  Main CFD Forum  1  August 19, 2006 12:33 
Test Case  ganesh  Main CFD Forum  0  March 16, 2006 12:34 
Looking for test case  William M.  Main CFD Forum  2  May 26, 2005 03:45 
test case?  lsm  Main CFD Forum  0  June 14, 2004 11:39 
test case  Follet  Main CFD Forum  0  July 8, 2002 04:07 