
[Sponsors] 
April 11, 2011, 02:46 

#21 
Senior Member
Mads Reck
Join Date: Aug 2009
Location: Copenhagen, Denmark
Posts: 175
Rep Power: 11 
Hi Felix,
sorry for the late reply and thanks a bunch for your kind and fast help. I know that José is working on it, using your suggestions, and we will report back with the outcome. Thanks again, Mads
__________________
Online free airfoilmesher for OpenFOAM here 

April 14, 2011, 03:43 

#22 
Member
José
Join Date: Jan 2011
Posts: 73
Rep Power: 8 
Hi Felix,
As Mads just said sorry for being so late to give you an answer. What I had wrong was the fvSolution file. Some of the tolerances were quite high that OF could not solve the equations correct and this is why it was taking so long time. Furthermore, since the equations are solved better I don´t have this strange behavior on the drag curve for the NACA0012 I sent to you some time ago. Thank you very much for all your help. It has really helped for the work I am doing in the thesis. Best regards, José 

April 14, 2011, 04:22 

#23 
Senior Member
Felix L.
Join Date: Feb 2010
Location: Hamburg
Posts: 165
Rep Power: 11 
Hello, José,
I'm glad to hear that your problem is solved and I could be of help. Feel free to ask anytime when there are new problems showing up (but which I really hope they don't). Good luck with your thesis! Greetings, Felix. 

May 17, 2011, 03:44 

#24 
New Member
Jordi Muela
Join Date: Mar 2011
Posts: 27
Rep Power: 9 
Hi everyone,
I'm validating a model to use it for find the Cd values of different geometries at different Re. Now I'm using a sphere due that is a geometry with a lot of experimental data. I'm having similar problems to those mentioned in this thread, so please, can someone post the files fvSolution and fvSchemes which works fine? I already tested all the suggestions explained in this thread but i couldn't obtain a good solution yet, my p residual it's still to high (and velocity residuals too...) Thanks a lot, Jordi. 

May 17, 2011, 03:54 

#25 
Member
José
Join Date: Jan 2011
Posts: 73
Rep Power: 8 
Hi Jordi,
I post the fvSolution and fvSchemes files which work fine for what I am doing (flow around an airfoil). What it really helped to me when I had convergence issues is to decrease the tolerance of all the residuals to a very low value (i.e. one value that none of them is getting >1e16). But, what do you consider high for the residuals? I am getting residuals for the pressure equation around 1e4. And the time of the computations when the airfoil is in the stall region is still high. If you get any new things regarding this thread, plesease, keep me/us posted. Greetings, José 

May 17, 2011, 05:21 

#26 
New Member
Jordi Muela
Join Date: Mar 2011
Posts: 27
Rep Power: 9 
Hi Jose,
first of all thanks for your fast reply! Just now i'm running a case with komegaSST model and for the moment, the behaviour seem 'better' than my previous cases, where i used the realizableKE model (Take a look to this report: http://citeseerx.ist.psu.edu/viewdoc...=rep1&type=pdf). Well, when my current simulation finish, then I test the 'fvSchemes' and 'fvSolution' that you attached and report here how it gone! (Now i'm using the 'fvSchemes' and 'fvSolution' files of the motorBike test case). With realizableKE I obtained residuals for p arround 1e2~1e3 (very high values...) but my tolerance and relTol values were highs too (arround 1e5~1e6 for tolerance...), but if I switch this values for others lower then i have divergence problems... Well, I'll keep you updated about my progress! Jordi. 

May 19, 2011, 06:23 

#27 
New Member
Jordi Muela
Join Date: Mar 2011
Posts: 27
Rep Power: 9 
Hi José,
after few simulations changing some parameters, turbulent model and mesh, I've arrived at the conclusion that my principal problem is the mesh. Now i'm getting reasonable results with a mesh where I refined the wake zone. I'm getting this results with the realizableKE model, the kOmegaSST model isn't working much well for me... Although i'm still having residuls for p around 1e2 ~ 1e3 (and I'm worried about that, but the results seems to match reasonably with the experimental..) Thanks a lot for your help! Jordi. 

June 7, 2011, 05:47 

#28 
Member
José
Join Date: Jan 2011
Posts: 73
Rep Power: 8 
Dear all,
I have tried to improve the speed of the computations done. I am doing simulations around a 2D airfoil (NACA0012) at Re=3.000.000 using the turbulence model kw SST and a mesh of 123.000 cells. I have tested how the convergence speed is modified by changing relTol (from fvSolution). I have used relaxation factor for the pressure equation=0.2 and relaxation factor for the velocity equation=0.8 since I tested once for another airfoil and this is the best I got. You can see the fvSolution file used I have tested it for relTol=0.001, relTol=0.01 and relTol=0.1, the cases converge in 5, 4 and 6 hours respectively. A case with the same mesh run with ANSYS CFX (using the double precission solver!) takes about 1 hour to converge. I still have to try it using GAMG solver for the pressure equation and see if I can improve it more... Doe anybody can give me any comment about this? Any improvement to this is very welcome! Thanks. Regards, José 

July 15, 2011, 10:40 

#29 
Senior Member
Guilherme da Silva
Join Date: Aug 2010
Location: Sao Paulo  Brazil
Posts: 104
Rep Power: 9 
Hello All,
Have you (Mads, José, Felix and Jordi) solved the issue? Do you all have an update? I am very interested to have the system files and/or the mesh itself. Just for your information, I saw a huge difference in convergence between OF1.7.1 and OF1.6ext. The latter had a much better convergence history/duration and result. It may be related to some differences in linear solvers implemented by Jasak and others from extended project. See some preview of the results at the thread below: http://www.cfdonline.com/Forums/ope...tml#post307393 Regards, Guilherme da Silva  ATS4i 

July 18, 2011, 02:57 

#30 
Senior Member
Mads Reck
Join Date: Aug 2009
Location: Copenhagen, Denmark
Posts: 175
Rep Power: 11 
Hi Guilherme da Silva,
we don't have any significant to add to the above, still OF is much slower (wall clock) than CFX 13 (and other codes I have tested) in terms of getting a final converged solution. Apart from that I am very happy with OpenFOAM 1.7.1 results on 2D airfoils (both normal thin ones and more exotic ones) with and without laminarturbulent transition modelling (with, thanks to Felix). Interesting information you have about the 1.7.1 and the 1.6ext convergence difference, I wonder if 2.0 is better than 1.7.1, we haven't tested that yet, but maybe someone else did? There must be a lot of revisions since they went past 1.8 and 1.9 :P Please update us if you find more on this issue BR Mads
__________________
Online free airfoilmesher for OpenFOAM here 

July 19, 2011, 11:32 

#31  
Senior Member
Felix L.
Join Date: Feb 2010
Location: Hamburg
Posts: 165
Rep Power: 11 
Hello, All,
I too don't have anything new to add to the above. Unfortunately I didn't have had much time lately to work with OpenFOAM, but at least I managed to upgrade to 2.0 and test a few things. I tried to reproduce the NASA NACA0012 validation test cases ( http://turbmodels.larc.nasa.gov/naca0012_val.html ) using the grids they provided. The cases ran well, but I'm unhappy with the results, because I'm not able to get into the asymptotic range with the force coefficients at alpha=0°. That kind of bothers me and I need to look deeper into it at some time, but for now you can have my systems directory  I don't think you'll find anything new there, though. Quote:
Greetings, Felix 

July 19, 2011, 11:33 

#32 
Senior Member
Felix L.
Join Date: Feb 2010
Location: Hamburg
Posts: 165
Rep Power: 11 
Oh by the way, here's the systemDirectory!


October 29, 2015, 12:27 

#33  
Senior Member
Join Date: Mar 2015
Posts: 249
Rep Power: 5 
Hello all, and thank you for this very interesting dicussion.
Felix, what made you choose the SpalartAllmaras model? I thought I read somewhere it is better to choose the kOmegaSST model for high AoAs. Has someone compared these two? Best regards, Kate Quote:


Tags 
2d, airfoil, cfx, convergence, openfoam 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Low Speed Airfoil  Mancusi  FLUENT  7  April 3, 2014 06:11 
CFX11 + Fortran compiler ?  Mohan  CFX  20  March 30, 2011 18:56 
[GAMBIT] Meshing airfoil using .dat file problem  creggie  ANSYS Meshing & Geometry  10  June 27, 2010 19:24 
Modeling Backflow for a 3D Airfoil (Wing of Finite Span)  Josh  CFX  9  August 18, 2009 11:31 
Airfoil boundary condition  Frank  Main CFD Forum  1  April 21, 2008 18:36 