
[Sponsors] 
September 11, 2007, 23:55 
Vincent, BastiL,
I just sen

#41 
New Member
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8 
Vincent, BastiL,
I just sent you the whole model via yousendit.com. Just go to the link that you will get on email accounts in the profile and download the file. thanks  Rajneesh 

September 12, 2007, 03:09 
Thanks a lot Rajneesh, I recei

#42 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9 
Thanks a lot Rajneesh, I received it.
I just had a look at your mesh and it's totaly different from mine, so it will be very interesting. I'm going to run it to see what I get, and I'll post my results. Regards, Vincent 

September 12, 2007, 03:35 
I can not try 1.4 at the momen

#43 
Senior Member
BastiL
Join Date: Mar 2009
Posts: 485
Rep Power: 11 
I can not try 1.4 at the moment, I am using simpleFoam 1.4.1 and I get:
Starting time loop Time = 1 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.0254472, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.00714854, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.0269422, No Iterations 1 DICPCG: Solving for p, Initial residual = 1, Final residual = 0.00938556, No Iterations 13 time step continuity errors : sum local = 38.8664, global = 1.26956, cumulative = 1.26956 DILUPBiCG: Solving for epsilon, Initial residual = 0.999636, Final residual = 0.0488436, No Iterations 1 bounding epsilon, min: 316.208 max: 3.94271e+06 average: 149.224 DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 7.80029e05, No Iterations 1 ExecutionTime = 215.08 s ClockTime = 215 s ... Time = 4 DILUPBiCG: Solving for Ux, Initial residual = 0.123077, Final residual = 0.00151918, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.291113, Final residual = 0.00156297, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.539444, Final residual = 0.000117586, No Iterations 1 DICPCG: Solving for p, Initial residual = 0.646448, Final residual = 0.00622016, No Iterations 59 time step continuity errors : sum local = 17.5265, global = 0.715884, cumulative = 0.36078 DILUPBiCG: Solving for epsilon, Initial residual = 0.0334807, Final residual = 4.11484e05, No Iterations 1 DILUPBiCG: Solving for k, Initial residual = 0.233191, Final residual = 0.000210396, No Iterations 1 ExecutionTime = 870.11 s ClockTime = 870 s .... Time = 9 DILUPBiCG: Solving for Ux, Initial residual = 0.147892, Final residual = 1.23908e07, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.414654, Final residual = 1.23514e06, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.51769, Final residual = 1.05291e06, No Iterations 1 DICPCG: Solving for p, Initial residual = 0.597334, Final residual = 0.00588535, No Iterations 23 time step continuity errors : sum local = 7.93123e+08, global = 3.50323, cumulative = 12.0621 DILUPBiCG: Solving for epsilon, Initial residual = 0.0486521, Final residual = 0.00112071, No Iterations 1 bounding epsilon, min: 1.14166e+14 max: 1.22753e+25 average: 2.34251e+19 DILUPBiCG: Solving for k, Initial residual = 0.611983, Final residual = 9.01935e06, No Iterations 1 bounding k, min: 3.57866e+09 max: 3.03393e+19 average: 3.13484e+13 ExecutionTime = 1790.34 s ClockTime = 1791 s ... Time = 12 DILUPBiCG: Solving for Ux, Initial residual = 0.00277457, Final residual = 3.62285e05, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.00162991, Final residual = 4.10471e05, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.00264718, Final residual = 4.61501e05, No Iterations 1 #0 Foam::error::printStack(Foam:stream&) in "/home/brblo/OpenFOAM/OpenFOAM1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/home/brblo/OpenFOAM/OpenFOAM1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #2 __restore_rt in "/lib64/tls/libc.so.6" #3 Foam::DICPreconditioner::calcReciprocalD(Foam::Fie ld<double>&, Foam::lduMatrix const&) in "/home/brblo/OpenFOAM/OpenFOAM1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #4 Foam::DICPreconditioner::DICPreconditioner(Foam::l duMatrix::solver const&, Foam::Istream&) in "/home/brblo/OpenFOAM/OpenFOAM1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #5 Foam::lduMatrix::preconditioner::addsymMatrixConst ructorToTable<foam::dicprecond itioner>::New(Foam::lduMatrix::solver const&, Foam::Istream&) in "/home/brblo/OpenFOAM/OpenFOAM1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #6 Foam::lduMatrix::preconditioner::New(Foam::lduMatr ix::solver const&, Foam::Istream&) in "/home/brblo/OpenFOAM/OpenFOAM1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #7 Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/brblo/OpenFOAM/OpenFOAM1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so" #8 Foam::fvMatrix<double>::solve(Foam::Istream&) in "/home/brblo/OpenFOAM/OpenFOAM1.4.1/lib/linux64GccDPOpt/libfiniteVolume.so" #9 main in "/home/brblo/OpenFOAM/OpenFOAM1.4.1/applications/bin/linux64GccDPOpt/simpleFoam " #10 __libc_start_main in "/lib64/tls/libc.so.6" #11 Foam::regIOobject::readIfModified() in "/home/brblo/OpenFOAM/OpenFOAM1.4.1/applications/bin/linux64GccDPOpt/simpleFoam " Floating point exception I tried to play around with relaxation factors and nonorthogonal correcors without success. I would be very happy if a FOAM expert could give me some hints. As mentioned before checkMesh reports some errors but other solvers run on this mesh without problems. Thanks 

September 12, 2007, 03:50 
Hi Bastil,
As I allready sa

#44 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9 
Hi Bastil,
As I allready said , I got the same problems. What I didn't mentioned earlier is that my mesh was also running fine with other solvers but not with OpenFOAM (1.4.1 at least). So I guess it's really a problem of stability with respect to cell shape. By the way, is your mesh refined a lot at the wall? Because I also noticed that simpleFoam doesn't really like very refined meshes at walls. I would also be interested in openfoam expert solution toughts on the subject. Vincent 

September 12, 2007, 04:28 
At first, you can try to start

#45 
Senior Member
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 217
Rep Power: 9 
At first, you can try to start from the potential solution.
Then, you can try switching off any turbulence model, at the beginning. After a few iteration, switch it on again, starting from the laminar solution. Good luck! Francesco 

September 12, 2007, 05:52 
Vincent: I have two prims laye

#46 
Senior Member
BastiL
Join Date: Mar 2009
Posts: 485
Rep Power: 11 
Vincent: I have two prims layers near the walls. I do not know if this is "very refined". But in every case it is a mesh suitable for turbulence model + wall function.
Francesco: Thanks for these hints. I will try to turn off turbulence first, maybe this will help. Bastil 

September 12, 2007, 19:54 
BastiL,
I had better succes

#47 
New Member
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8 
BastiL,
I had better success with GAMG solver for pressure. See it in the setup files I posted in this thread. Also, see if your initial k and eps values are reasonable  R 

September 13, 2007, 02:52 
Rajneesh,
I agree. I get be

#48 
Senior Member
BastiL
Join Date: Mar 2009
Posts: 485
Rep Power: 11 
Rajneesh,
I agree. I get better results with the settings from Hrv: http://www.cfdonline.com/OpenFOAM_D...es/1/4245.html Nevertheles in 1.4.1 use GAMG instead of AMG. I have 68 Timesteps so far and it looks much better. I will keep you up. 

September 13, 2007, 05:27 
Hi everybody,
did someone t

#49 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9 
Hi everybody,
did someone tried to change the liftDrag utility to account for turbulence. I mean replacing dragCoefficient(...) by turbDragCoefficient(...). I face a stupid problem. For the turbDragCoefficient computation, one need to pass the turbulence model since the first function argument is: const autoPtr<turbulencemodel>& turbulence my question is what should I add to liftDrag.C to pass this turbulence model? Thanks in advance. Vincent 

September 13, 2007, 10:42 
I had written time ago this ap

#50 
Member
Rosario Russo
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 56
Rep Power: 8 
I had written time ago this application which computed at runtime the forces on a body. It is not too efficient but it should work.
It runs by this command: ssimpleFoam <root> <case> "(patch1 patch2 patch3)" where patch13 are the patches of the body you want to calculate the force on. I run it in version 1.3 but it I verified it works with 1.4 as well (I don't have installed 1.4.1). Hope this is useful. ssimpleFoam.tgz to Rajneesh: I had a quick look at the setting of the Amhmed body you posted. How did you choose turbulent parameters? I mean k and epsilon at inlet. Why did you start by zero velocity as initial condition? 

September 13, 2007, 23:13 
Rosario,
Initially I had pi

#51 
New Member
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8 
Rosario,
Initially I had picked values corresponding to the turbulence intensity of 0.6 and length scale of 0.02. It gives k and eps of order of 0.1. After that I played with several other values. Simulation does blow up if these values are too much out of reasonable limits. There is no particular reason for starting from 0. Just thats the way I have been doing at my work for Fluent simulations. This choice seems safest even though it may take little longer to converge for some cases. 

September 14, 2007, 10:46 
Thank you Rajneesh for your an

#52 
Member
Rosario Russo
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 56
Rep Power: 8 
Thank you Rajneesh for your answer.
Actually I was thinking to use an higher value for turbulence intensity, but I don't know the details of the ahmed body experiment. Are your result affected much by the turbulence set at inlet? (I'm just curious). 

September 17, 2007, 04:25 
Hi Rajneesh,
I come back t

#53 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9 
Hi Rajneesh,
I come back to you after I run your case. I didn't change anything and the computation went fine to the end. Now I would like to compute the lift and drag and I get some strange results. Here is what I get from my liftDrag utility: Create mesh for time = 1500 Time = 1500 Reading U Reading p Reading/calculating face flux field phi Selecting incompressible transport model Newtonian Selecting turbulence model RNGkEpsilon Inlet velocity: (60 0 0) pressure Coefficient: 0.00540718 viscous Coefficient: 0.000145663 turb Coefficient: 0.00139343 Wall patch 3 named a.forebody : Reference area: 1 Reference length: 0.182 Total Turbulent drag coefficient: 0.00415941 Lift coefficient: (0 0.0314594 0.00310949) pressure Coefficient: 1.42641e12 viscous Coefficient: 0.000213444 turb Coefficient: 0.000637851 Wall patch 4 named a.side : Reference area: 1 Reference length: 0.862199 Total Turbulent drag coefficient: 0.000424407 Lift coefficient: (0 0.0411145 8.50987e07) pressure Coefficient: 2.85131e07 viscous Coefficient: 0.000111487 turb Coefficient: 0.000347901 Wall patch 5 named a.top : Reference area: 1 Reference length: 0.645392 Total Turbulent drag coefficient: 0.000236699 Lift coefficient: (0 3.45158e06 0.0261528) pressure Coefficient: 0 viscous Coefficient: 0.000150484 turb Coefficient: 0.00048029 Wall patch 6 named a.bot : Reference area: 1 Reference length: 0.862 Total Turbulent drag coefficient: 0.000329805 Lift coefficient: (0 1.36859e07 0.0361365) pressure Coefficient: 0.00288352 viscous Coefficient: 3.65491e05 turb Coefficient: 4.66086e05 Wall patch 7 named a.baklite : Reference area: 1 Reference length: 0.216612 Total Turbulent drag coefficient: 0.00287346 Lift coefficient: (0 1.51287e06 0.0129836) pressure Coefficient: 0.0133659 viscous Coefficient: 3.91805e07 turb Coefficient: 0.000242045 Wall patch 8 named a.rear : Reference area: 1 Reference length: 0 Total Turbulent drag coefficient: 0.0136083 Lift coefficient: (0 1.37909e05 5.13891e06) One thing to notice is that I prescribe a reference area of 1mē. So the numbers have to be divided by the real frontal area of the ahmed body which in your case is 0.5x0.288x0.389 (because it's a half body,am I right?). So, to obtain the pressure coefficient for instance, I sum all pressure coefficients of each body part and divide by the number explained above. Then I get a rounded pressure coefficient of 0.387 which is exactly twice as yours. The same can be done with the viscous coefficient and I obtain 0.012 which is also twice as yours. My questions are then, are your drag coefficients computed using the half body frontal area or the whole frontal area? are my computations wrong? Where is my mistake? Thans a lot for your help. Regards, Vincent 

September 17, 2007, 09:33 
Vincent,
Its quite possible

#54 
New Member
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8 
Vincent,
Its quite possible that I am using area for the full body. We have to use the half model frontal area, exactly as you mentioned. I will check it from home tonight and let you know I had modifed the computeForces.H program by hardcoding the area value (full body area = 0.1120). I have been lately using full model as well to see if the symmetry assumption makes any difference. The Fluent setup that predicted Cd exactly for 12.5 deg body is way off for this 30 deg model. BTW if you are interested here is full mesh model for 30 Deg Ahmad body.It should be available on this link for next twothree days. http://download.yousendit.com/09F309E86E2932AB Rosario: I was playing with various turbulence conditions to see if the solution converges or blows up. I never really ran it long enough to get final values. All: I am still trying to figure out best schemes for the second order accuracy for external aero simulations. Please post your observations.  Rajneesh 

September 17, 2007, 10:59 
Ok, so I guess the drag coeffi

#55 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9 
Ok, so I guess the drag coefficient you gave before in this thread should be multiplied by 2.
This actually closer to the results I get by using my own mesh. Unfortunately this is not a good news since it is twice as large as ahmed results. And this factor 2 is very disturbing. I'm going to download you 30° mesh and run it to see if we obtain the same results (i.e. drag coefficient twice as large as ahmed for a 30° slant angle). Anyway thanks a lot for sharing your work. Vincent 

September 18, 2007, 00:00 
Yes, confirmed I was using are

#56 
New Member
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8 
Yes, confirmed I was using area of the full model.
So Sorry for the confusion. By changing to second order schemes, Pressure Cd does come down to 0.320 (with correct area) but it is still quite far from the experimental values.  R 

September 18, 2007, 04:53 
Hi all,
I started working o

#57 
Senior Member
BastiL
Join Date: Mar 2009
Posts: 485
Rep Power: 11 
Hi all,
I started working on the half model from Rajneesh yesterday.First calculations went fine. Concerning the differences we should consider the following (I do not have th evalues of th ehmed experiment...) 1.) Make sure drag/lift is computed correct. Which tools are you using? I can not find any of the draglift tools in OF 1.4.1, are they? Where can I get them? 2.) Get rid of meshdependencies concerning near wall resolution and farfield. I guess mesh from Rajneesh is nice but hexcore mesh would be nicer. Also wake and stagnation point refinements are the key to validation. 3.) Turbulence modelling is another key. BastiL 

September 18, 2007, 05:54 
Hi everybody,
So, unfortuna

#58 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9 
Hi everybody,
So, unfortunatly I was right, the drag coefficients were wrong. But as you said, Rajneesh, by changing fvSchemes we get closer to the right values. Actually I changed the schemes to these ones: ddtSchemes { default steadyState; } gradSchemes { default fourth; grad(p) fourth; grad(U) fourth; } divSchemes { default none; div(phi,U) Gauss SFCD; div(phi,k) Gauss SFCD; div(phi,epsilon) Gauss SFCD; div(phi,R) Gauss SFCD; div(R) Gauss SFCD; div(phi,nuTilda) Gauss SFCD; div((nuEff*dev(grad(U).T()))) Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A(U)),p) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; laplacian(DREff,R) Gauss linear corrected; laplacian(DnuTildaEff,nuTilda) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default corrected; } and I'm getting a value of 0.27 (using th right area) for the drag coefficient which is not so bad. I'm still playing with the schemes to find the best ones to use. Then, we'll have to find the best turbulence model to see if we get better results as Bastil has mentioned. For the liftDrag utility, I use one I found on this forum. Use the search command to find the thread, there is an explanation on how to install the liftDrag tool on previous version of OpenFOAM (and this also works with 1.4.1). Vincent 

September 18, 2007, 16:18 
A good news I guess
Fluent si

#59 
New Member
Rajneesh
Join Date: Mar 2009
Posts: 28
Rep Power: 8 
A good news I guess
Fluent simulation for the same mesh (0.63 Mill Cells) as used for OpenFoam predicts Cd of 0.309. Now OF results do not look that bad. Fluent model of ~3 Mill cells gives same result as test. I will try that on my machine sometime soon. From now on, I will be uploading interesting results, flow vis comparisons to the googlepage site linked in my profile. 

September 18, 2007, 16:53 
Actually, yes, it looks like a

#60 
Senior Member
Vincent RIVOLA
Join Date: Mar 2009
Location: France
Posts: 281
Rep Power: 9 
Actually, yes, it looks like a good news.
I didn't understand how OpenFOAM was so far from Fluent, but the mesh difference is certainly one of the reasons. I'm waiting forward to see what you get. I'll keep you updated if I find better results with other shemes. 

Thread Tools  
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 13:34 
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 