Hi, I got some weird proble
I got some weird problems the other days. First of all, when I start from an steady simple result and switch to turbFoam or transientFoam. The time step is printed out as an integer and does not enlarge, when I use a small time step. I used the controlDict from the tutorial/turbfoam. I was thinking that it depends on the 'application' setting in the controlDict, but it does not change!?
A somewhat similar problem occurs when starting the simulation. E.g. renaming the 'steady' directory from '300' to '300.0' and setting the start time to '300.0' openfoam still tries to read the '300' directory!? It actually happens with oodles, transientSimple and turbFoam. Maybe anyone had similar problems before?
Another weird problem occurs, when running a polyhedral mesh room (3Mio cells) in parallel on a nec cluster with pbs queueing. The calculation of the CFL number is way to high, about 1*10^12 for a time step of 0.000001 as a mean, but in serial it is around 1*10^-2. In addition I am pretty sure the oodles run in parallel worked out before (with just the above mentioned time print problem); unfortunately I overwrote the log file. I am using version 1.4.1 and 'just' adjusted openmpi with support of pbs (--with-tm) and infiniband (--with-mvapi). Could this have an effect at all?
Below is the first try on a lo
Below is the first try on a local machine in serial. As you see the time steps are still integers using a time step of: 'deltaT 0.000001'; the CFL look like expected:
Time = 550
Courant Number mean: 0.000139222 max: 0.042469
DILUPBiCG: Solving for Ux, Initial residual = 9.28159e-05, Final residual = 9.06085e-10, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 7.53042e-05, Final residual = 2.06212e-09, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.00010302, Final residual = 6.90042e-10, No Iterations 1
GAMG: Solving for p, Initial residual = 0.00185969, Final residual = 4.83616e-09, No Iterations 10
time step continuity errors : sum local = 4.47401e-16, global = 2.32446e-17, cumulative = -2.25216e-12
GAMG: Solving for p, Initial residual = 9.58305e-05, Final residual = 9.09056e-09, No Iterations 6
time step continuity errors : sum local = 8.40314e-16, global = 2.88236e-17, cumulative = -2.25213e-12
ExecutionTime = 17959.2 s ClockTime = 18053 s
Time = 550
Courant Number mean: 0.000139217 max: 0.042348
A similar calculation was done on cluster with the same time step and on 16 cpus:
9 Exec : oodles . E1_POLY_3Mio
10 Date : Feb 18 2008
11 Time : 17:15:24
12 Host : noco205.nec
13 PID : 32332
14 Root : /scratch2/ws/ppb367-E1_POLY_3Mio_LES-0
15 Case : E1_POLY_3Mio
16 Nprocs : 1
17 Create time
19 Create mesh, no clear-out for time = 3800
21 Reading field p
23 Reading field U
25 Reading/calculating face flux field phi
27 Selecting incompressible transport model Newtonian
28 Creating field Umean
30 Creating field R
32 Creating field Bmean
34 Creating field epsilonMean
36 Creating field pMean
38 Creating field pPrime2Mean
41 Starting time loop
43 Time = 3800
45 Courant Number mean: 1.55462e+08 max: 3.75517e+12
46 #0 Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&) in "/app/pag/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
This is pretty strange; at least for me!?
Using transientSimple I get the above mentioned problem as well:
2 Time = 3800.03
674 Courant Number mean: 2.81951e+11 max: 6.79852e+15
675 DILUPBiCG: Solving for Ux, Initial residual = 0.00503398, Final residual = 5.36932e-05, No Iterations 1
676 DILUPBiCG: Solving for Uy, Initial residual = 0.00521737, Final residual = 0.000267142, No Iterations 1
677 DILUPBiCG: Solving for Uz, Initial residual = 0.00482197, Final residual = 3.16431e-05, No Iterations 1
678 GAMG: Solving for p, Initial residual = 0.0545565, Final residual = 4.68516e-08, No Iterations 26
679 time step continuity errors : sum local = 874.245, global = -0.804416, cumulative = -112.988
680 DILUPBiCG: Solving for Ux, Initial residual = 0.00503979, Final residual = 5.39757e-05, No Iterations 1
681 DILUPBiCG: Solving for Uy, Initial residual = 0.00522042, Final residual = 0.000267125, No Iterations 1
682 DILUPBiCG: Solving for Uz, Initial residual = 0.00482468, Final residual = 3.16486e-05, No Iterations 1
683 GAMG: Solving for p, Initial residual = 0.0541601, Final residual = 5.76659e-08, No Iterations 26
684 time step continuity errors : sum local = 1093.39, global = -2.69242, cumulative = -115.681
685 DILUPBiCG: Solving for omega, Initial residual = 0.00643001, Final residual = 0.000111815, No Iterations 1
686 DILUPBiCG: Solving for k, Initial residual = 0.0159787, Final residual = 0.000204375, No Iterations 1
687 ExecutionTime = 2778.71 s
690 Time = 3800.03
692 Courant Number mean: 2.87402e+11 max: 6.93128e+15
693 DILUPBiCG: Solving for Ux, Initial residual = 0.0050327, Final residual = 5.38822e-05, No Iterations 1
694 DILUPBiCG: Solving for Uy, Initial residual = 0.00521864, Final residual = 0.000267173, No Iterations 1
695 DILUPBiCG: Solving for Uz, Initial residual = 0.00481974, Final residual = 3.16345e-05, No Iterations 1
696 GAMG: Solving for p, Initial residual = 0.0544617, Final residual = 6.53602e-08, No Iterations 26
697 time step continuity errors : sum local = 1245.95, global = -2.68424, cumulative = -118.365
698 DILUPBiCG: Solving for Ux, Initial residual = 0.00503713, Final residual = 5.41075e-05, No Iterations 1
699 DILUPBiCG: Solving for Uy, Initial residual = 0.00522195, Final residual = 0.000266228, No Iterations 1
700 DILUPBiCG: Solving for Uz, Initial residual = 0.00482254, Final residual = 3.16432e-05, No Iterations 1
701 GAMG: Solving for p, Initial residual = 0.0543004, Final residual = 8.99008e-08, No Iterations 25
702 time step continuity errors : sum local = 1723.18, global = -3.39244, cumulative = -121.757
703 DILUPBiCG: Solving for omega, Initial residual = 0.00646512, Final residual = 0.000111878, No Iterations 1
704  #0 Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&) in "/app/pag/OpenFOAM/OpenFOAM-1.4.1/lib/linux64GccDPOpt/libOpenFOAM.so"
Domain bounding box: (0.400533 -0.805 0.105) (3.59 0.805 1.32)
Boundary openness (-8.03796e-17 0 -8.03796e-17) OK.
Max cell openness = 1.93479e-16 OK.
Max aspect ratio = 8.71581 OK.
Minumum face area = 8.02934e-09. Maximum face area = 0.000233939. Face area magnitudes OK.
Min volume = 6.05927e-12. Max volume = 6.1045e-06. Total volume = 2.84135. Cell volumes OK.
Mesh non-orthogonality Max: 70.3753 average: 13.8218
*Number of severely non-orthogonal faces: 2.
Non-orthogonality check OK.
<<Writing 2 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 3.80142 OK.
Min/max edge length = 8.70872e-05 0.0161572 OK.
*There are 2510 faces with concave angles between consecutive edges. Max concave angle = 90 degrees.
<<Writing 2510 faces with concave angles to set concaveFaces
Face flatness (1 = flat, 0 = butterfly) : average = 0.98761 min = 0.655516
*There are 171 faces with ratio between projected and actual area < 0.8
Minimum ratio (minimum flatness, maximum warpage) = 0.655516
<<Writing 171 warped faces to set warpedFaces
Probably, I am doing something stupid... Any ideas?
Your time is printed with (usu
Your time is printed with (usually) 6 digits precision. Increase in the controlDict the writePrecision and also timePrecision to 15 (significant number of digits for doubles). And write results binary.
Redecompose (decomposePar -fields) the time you restart the serial run from and try again so you have exactly the same situation.
Hi Mattijs, thanks for your
thanks for your advice! But this would not correct the cfl numbers, does it!? It's a polyhedral ccm+ mehs with a minimum cell size of the order of 10^-12 , the max. velocity is around 3m/s. A time step of 1sec gives a max. Courant of 2900 testing it with starccm+. So with my little time step of 0.000001 the first calculated OpenFoam number of around 0.04 looks good. Is there anything else going wrong or is setting the digits precision enough? I'll try it as soon as some cpus are available...
Hi Mattijs, it works :-) Th
it works :-) Thanks for your help!
I am facing a problem during solving. I am using the k-w SST turbulence model and during iteration, I have both bounding k and omega. The min and max values are between 1e-6 to 1e+6.
FYI, I applied boundary layers on my car (it's an external aerodynamics of car in a wind tunnel case) - about 10 layers and the y+ values are between 0 to 100 (average of about 30).
I think it is because of my y+ values but I am not really sure. If it's true, then should I increase my y+ values by making the layers nearest to wall to be thicker?
Could you help & advise me on this?
|All times are GMT -4. The time now is 21:03.|