
[Sponsors] 
April 18, 2012, 08:57 

#41 
Member
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 7 

Sponsored Links 
April 18, 2012, 21:56 

#42 
Member
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 7 
Here is the mesh that I'm currently using:
A friend of mine made it in gridgen and saved it in the openFOAM format. I ran Code:
autoPatch 90 > log.autoPatch Here is the mesh closerup: The leading edge: The trailing edge: Residuals: Force coefficients: Velocity: Pressure: nuTilda: Everything looks good aside from the fact that my drag coefficient is still not matching with Abbot and Von Doenhoff. All coefficients are off by a factor of 10 since I didn't change the reference length or area with this new mesh, but even adjusting for that the drag coefficient is still off (I'm getting 0.014ish where I expect .008ish). This is still with the SpalartAllmaras model. I will try this with some different boundary conditions (different from those in the attached files) and then try a different turbulence model (kepsilon maybe?). I'll keep updating this thread. http://dl.dropbox.com/u/62138912/nut http://dl.dropbox.com/u/62138912/nuTilda http://dl.dropbox.com/u/62138912/p http://dl.dropbox.com/u/62138912/U 

April 18, 2012, 22:31 
set a very thin patch

#43 
New Member
Qiang
Join Date: Mar 2012
Posts: 12
Rep Power: 7 

April 19, 2012, 04:30 

#44 
Member
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 8 
Hi Joe,
that seems to be a nice mesh. The first layer of cells in the boundary layer looks a bit too thick. Which is your y+? And which is the angle of attack you have simulated? By the way, as you know predicting satisfactorily the drag coefficient is much more difficult than predicting the lift. This means that you can probably improve a bit your simulation but I think you should not expect a perfect match with the drag measurements (at least for the stall region). Good luck Ivan Last edited by Ivanet; April 19, 2012 at 04:57. 

April 19, 2012, 04:55 

#45 
Member
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 8 
Hi Qiang Wang,
What I would do is to create a patch that corresponds exactly with your region of interest. You can do this e.g. dividing your stl in several parts before doing your mesh. If you mesh is already done, and you do not want to redo it, you could make the patch with createPatch (I have never tried that, but I guess it should work). Greetings Ivan 

April 19, 2012, 06:28 

#46  
Member
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 7 
Quote:
I'm still looking at an 8 degree angle of attack. The maximum y+ from the 0 timestep is 23.712  this isn't the complete picture though is it? I ran Code:
yPlusRAS I understand that I shouldn't expect a perfect match for drag, but I'm currently off by about 40%. I'd be happy with a 10% error, but I think 40% is too much. 

April 19, 2012, 06:40 

#47  
New Member
Qiang
Join Date: Mar 2012
Posts: 12
Rep Power: 7 
Quote:
I think I've got the point. Best regards, Qiang Wang 

April 19, 2012, 08:43 

#48 
Member
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 7 
Below are the boundary conditions for two cases I have run. The first case has the accurate lift coefficient and the 40% high drag coefficient with the results shown in my previous post. The second case has both lift and drag coefficients on the order of 1e+38, so I'm pretty sure that's incorrect. It was wrong on my part to change to many of the boundary conditions between these two cases since now I don't know which change in particular caused these ridiculous errors, so I'm going to have to go back and make systematic changes to figure out what's going on. Shooting from the hip I think it's the farfield boundary condition for pressure, but I don't know for sure. It may also be the change to the wall function in nut at the airfoil. I haven't done any postprocessing on the second case yet since I can only access text files from my phone so I only looked at forceCoeffs.dat.
Any ideas?


April 19, 2012, 09:16 

#49  
Member
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 8 
Quote:
Greetings Ivan 

April 19, 2012, 16:33 

#50 
Member
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 7 

April 20, 2012, 07:32 

#51 
Member
Join Date: Oct 2010
Location: Germany
Posts: 39
Rep Power: 8 
In that case it might be even too small. I think y+ should be between 30 and 200 for simulations with wall functions.
However I am not sure if you have calculated y+ or y*. Using yPlusRAS seems to give you in fact y*. For more info check for example this thread: http://www.cfdonline.com/Forums/ope...earstress.html Can anyone give a hint on this? Ivan 

April 20, 2012, 12:54 

#52 
New Member
Farshad Rezaei
Join Date: Apr 2012
Posts: 10
Rep Power: 7 

April 20, 2012, 13:13 
lift coefficient of NACA0012

#53 
New Member
Farshad Rezaei
Join Date: Apr 2012
Posts: 10
Rep Power: 7 
Hi
I've used simpleFoam to analyze NACA0012 Airfoil with Angle of Attack 5 degrees. turbulence model is smalartAllmaras. The lift coefficient is 0.476 after 5500 sec. the lift coefficient did not have a constant value, the largest amount of it was 0.5 in 2500 sec, but its value had been changed during the time and after 4100 sec the value of lift coefficient was the same about 0.47 and after 4100 sec it did not change. By using Thin Airfoil Theory, for angle of attack 5 degree, the lift coefficient is about 0.548 and I have 13% error. I don't know that what is my problem, is my lift coefficient good? 

April 20, 2012, 14:50 

#54  
Member
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 7 
Quote:


April 28, 2012, 17:18 

#55 
Member
Joe
Join Date: Dec 2011
Location: Groton, CT
Posts: 67
Rep Power: 7 
So I derange this at a Reynolds number an order of magnitude higher than before in order to get a larger y+. The drag is now much better, thanks for the suggestion Ivan. I think I've done this static problem to death now so I'm moving on to pimpleDyMFoam.


November 20, 2014, 23:02 
Naca 0012 (urgent)

#56 
New Member
Shravan
Join Date: Sep 2014
Posts: 4
Rep Power: 4 
Can anyone just give me the naca oo12 airfoil tabulated data of cl,cd at respective AOA


November 24, 2014, 14:28 
Request for help

#57 
Member
Gareth
Join Date: Jun 2010
Posts: 37
Rep Power: 9 
Hi there, i have been trying to model a sg6041 foil in openfoam.
Its a simple mesh done through snappyhexmesh with the foil inputed as a stl. I have split the foil into 4 sections and included a refinement box around the foil. My question is about the lift and drag... When i run simpleFoam for my case i get a CL = 0.1402 and a CD of 0.00646, which is to far off when compared to the same foil run through the xfoil program  xfoil reported CL = 0.287 and CD = 0.00407. I am using the KSST model with initial K = 1.19 and omega = 17.94 I run the simulation for 4000 iterations, and the last run of my log file is below Case info: Frestream velocity = 26.75m/s Re = 1779735 equates to kinematic viscosity = 1.5e5 Chord of 1m Depth of 0.1m The top and bottom patches are set to symmetry I have attached 2 images of my mesh, i will send the polymesh to anyone but i have no site to post it on and its too big for the forum... I have also attached my initial conditions and the forces file i use to calc CL and CD forcesDn are the lower half of the foil and forcesUp are the upper half. Finally forces T looks athe entire foil as does the coeff section. The split was a check on patch referencing i was doing. I cant figure out why the large difference in my coefficients. I am struggling with what seems to be a small issue for a while now and i think i am losing it.. Please any help is appreciated. __________________________________________________ _________ Time = 4000 smoothSolver: Solving for Ux, Initial residual = 1.02476e08, Final residual = 7.66026e10, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 9.04285e09, Final residual = 9.04285e09, No Iterations 0 GAMG: Solving for p, Initial residual = 1.49412e07, Final residual = 8.26346e09, No Iterations 1 time step continuity errors : sum local = 3.7976e10, global = 2.87202e12, cumulative = 0.000439424 smoothSolver: Solving for omega, Initial residual = 9.88073e09, Final residual = 9.88073e09, No Iterations 0 smoothSolver: Solving for k, Initial residual = 9.84067e09, Final residual = 9.84067e09, No Iterations 0 ExecutionTime = 66.76 s ClockTime = 67 s forces forcesUp output: sum of forces: pressure : (0.0762727 5.43847 9.67512e19) viscous : (0.0736868 0.00385495 1.43458e20) porous : (0 0 0) sum of moments: pressure : (0.679809 0.00953408 0.76145) viscous : (0.000481869 0.00921084 0.00687399) porous : (0 0 0) forces forcesDn output: sum of forces: pressure : (0.0213602 0.424607 2.4701e19) viscous : (0.0598335 0.00170402 4.72061e21) porous : (0 0 0) sum of moments: pressure : (0.0530759 0.00267002 0.345743) viscous : (0.000213003 0.00747919 0.00256536) porous : (0 0 0) forces forcesT output: sum of forces: pressure : (0.0976329 5.01386 7.20502e19) viscous : (0.13352 0.00215093 9.62519e21) porous : (0 0 0) sum of moments: pressure : (0.626733 0.0122041 1.10719) viscous : (0.000268866 0.01669 0.00430862) porous : (0 0 0) forceCoeffs forceCoeffs output: Cm = 0.000807592 Cd = 0.00646074 Cl = 0.140198 Cl(f) = 0.0709065 Cl(r) = 0.0692913 End __________________________________________________ _____________ 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
fluentMeshToFoam multidomain mesh conversion problem  Attesz  OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ...  12  May 2, 2013 10:52 
matching variable data with grid point data  anfho  OpenFOAM Programming & Development  0  May 6, 2011 15:28 
Naca0012 ke mpirun gives fpe whereas simpleFoam not  Pierpaolo  OpenFOAM  1  May 8, 2010 03:08 
NACA0012 Data as a function of Re for a VAWT model  psd  Main CFD Forum  1  July 31, 2009 22:04 
How to update polyPatchbs localPoints  liu  OpenFOAM Running, Solving & CFD  6  December 30, 2005 18:27 
Sponsored Links 