|
[Sponsors] |
Too much iterations for k, epsilon with Pointwise mesh |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
|
October 5, 2015, 03:51 |
Too much iterations for k, epsilon with Pointwise mesh
|
#1 |
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 10 |
Hello, Foamers
I'm trying to solve flow past a floating square box. The solver is interFoam(Multiphase water, air). The domain, suface mesh, volume mesh are generated by Pointwise and I set boundary conditions as below : Inlet, oulet, atmosphere : patch bottom, midplane, side : symmetry box : wall Volume mesh is composed of tetrahedron mesh. Mesh quality checked by checkMesh utility was fine with some skew cells. The problem is that Iterations for alpha.water and k, epsilon is 1000 and they blow up later... I already faced this situation when the mesh was structured mesh.. I thought unstructured mesh will be a solution for this situation but... nothing changed Here is terminal output Code:
Time = 0.000119976 smoothSolver: Solving for alpha.water, Initial residual = 2.10029456432146e-06, Final residual = 0.0004465071153368, No Iterations 1000 Phase-1 volume fraction = 0.626758885470715 Min(alpha1) = 0 Max(alpha1) = 2.51427683470041 MULES: Correcting alpha.water MULES: Correcting alpha.water MULES: Correcting alpha.water Phase-1 volume fraction = 0.626758885470664 Min(alpha1) = 0 Max(alpha1) = 2.5111203422983 GAMG: Solving for p_rgh, Initial residual = 1, Final residual = 0.000412756523842382, No Iterations 4 GAMG: Solving for p_rgh, Initial residual = 0.101705754512192, Final residual = 0.000100928301496662, No Iterations 4 time step continuity errors : sum local = 3.65937145748082e-07, global = 1.53699517734662e-08, cumulative = 1.53784861589855e-08 GAMG: Solving for p_rgh, Initial residual = 0.0312962317006745, Final residual = 1.39933880273081e-05, No Iterations 5 GAMG: Solving for p_rgh, Initial residual = 0.00996448307785306, Final residual = 7.62790351177124e-06, No Iterations 5 time step continuity errors : sum local = 3.52922607711308e-08, global = 7.58057755027101e-10, cumulative = 1.61365439140126e-08 GAMG: Solving for p_rgh, Initial residual = 0.00468422248968285, Final residual = 4.66016854885601e-06, No Iterations 5 GAMG: Solving for p_rgh, Initial residual = 0.00252317454590901, Final residual = 3.49969247968792e-08, No Iterations 12 time step continuity errors : sum local = 1.63507334863481e-10, global = 2.95406036297376e-12, cumulative = 1.61394979743756e-08 smoothSolver: Solving for epsilon, Initial residual = 0.0633688257280632, Final residual = 0.0632861832323256, No Iterations 1000 smoothSolver: Solving for k, Initial residual = 0.999999985453537, Final residual = 1.00589685637645, No Iterations 1000 ExecutionTime = 314.36 s ClockTime = 325 s Have anyone experienced this too much iteration problem? If so, how can I solve this problem? :confused: Best regards, tigger |
|
October 8, 2015, 09:17 |
|
#2 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
This is quite unusual... the linear solver doesn't converge at all.
Did you try to run a different solver for k and epsilon? Code:
"(U|k|epsilon|omega|UFinal|kFinal|epsilonFinal|omegaFinal)" { solver PBiCG; preconditioner DILU; tolerance 1e-12; relTol 1.0e-2; maxIter 100; };
__________________
The skeleton ran out of shampoo in the shower. |
|
October 10, 2015, 09:47 |
Thanks! Philipp
|
#3 | |
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 10 |
Quote:
I tried to use PBiCG solver you suggested Now the K, epsilon iterations become stable Code:
DILUPBiCG: Solving for alpha.water, Initial residual = 9.41257114753943e-07, Final residual = 6.69250718355886e-11, No Iterations 1 Phase-1 volume fraction = 0.626760378142215 Min(alpha1) = -1.16185071173307e-06 Max(alpha1) = 1.00150910236442 Applying the previous iteration compression flux MULES: Correcting alpha.water MULES: Correcting alpha.water MULES: Correcting alpha.water MULES: Correcting alpha.water Phase-1 volume fraction = 0.626760378142315 Min(alpha1) = -1.16185071173307e-06 Max(alpha1) = 1.00150901821138 GAMG: Solving for p_rgh, Initial residual = 0.000268113771479435, Final residual = 1.31199231523444e-07, No Iterations 5 GAMG: Solving for p_rgh, Initial residual = 8.9469043939113e-05, Final residual = 8.44752800100194e-08, No Iterations 5 time step continuity errors : sum local = 1.15163397615092e-11, global = -1.29175373620592e-12, cumulative = -1.64869290559949e-06 GAMG: Solving for p_rgh, Initial residual = 4.07512657567795e-05, Final residual = 3.94730642661602e-08, No Iterations 6 GAMG: Solving for p_rgh, Initial residual = 3.7833103278026e-05, Final residual = 3.70998267918502e-08, No Iterations 5 time step continuity errors : sum local = 5.07003233184369e-12, global = 7.53555301266291e-13, cumulative = -1.64869215204419e-06 GAMG: Solving for p_rgh, Initial residual = 1.44866320494826e-05, Final residual = 3.79502063541261e-08, No Iterations 4 GAMG: Solving for p_rgh, Initial residual = 1.19072340126574e-05, Final residual = 4.81493222880152e-08, No Iterations 3 time step continuity errors : sum local = 6.55465097078055e-12, global = -4.41939941264471e-13, cumulative = -1.64869259398413e-06 DILUPBiCG: Solving for epsilon, Initial residual = 0.000317455367614486, Final residual = 3.20877793792615e-07, No Iterations 2 DILUPBiCG: Solving for k, Initial residual = 8.09326775207824e-09, Final residual = 8.09326775207824e-09, No Iterations 0 ExecutionTime = 12857.71 s ClockTime = 13028 s You can see the residuals in attached picture. I have to find solutions for this situation.. Anyway, Thanks again! |
||
October 12, 2015, 07:14 |
|
#4 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
You need to post the log output of the blowup (and some iterations before)...
__________________
The skeleton ran out of shampoo in the shower. |
|
October 12, 2015, 07:17 |
|
#5 |
Senior Member
Jan
Join Date: Jul 2009
Location: Hamburg
Posts: 137
Rep Power: 19 |
Jason, I can't see the screenshots. Can you upload again?
|
|
October 12, 2015, 07:54 |
|
#6 |
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 10 |
Oops, I forgot to attach screenshot
Here it is Thanks, tigger |
|
October 12, 2015, 07:56 |
|
#7 |
Senior Member
Jan
Join Date: Jul 2009
Location: Hamburg
Posts: 137
Rep Power: 19 |
ok, can you do one more with mesh grid on?
|
|
October 12, 2015, 08:25 |
|
#8 |
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 10 |
|
|
October 12, 2015, 07:53 |
|
#9 | |
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 10 |
Quote:
Actually, I stopped the calculation because the residual is getting weird.. Thanks, tigger |
||
October 12, 2015, 08:04 |
|
#10 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
Can you post the fvSchemes and fvSolution that you used for to get that log output?
__________________
The skeleton ran out of shampoo in the shower. |
|
October 12, 2015, 08:22 |
|
#11 |
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 10 |
Here it is
|
|
October 12, 2015, 08:34 |
|
#12 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
Several things:
1) You did not change the laplacian scheme to uncorrected. 2) You should use numerically safe settings for the other schemes as well, such as "Gauss upwind" instead of linearUpwind and vanLeer. If they work, you can start to introduce better schemes, one by one. 3) Using p_rghFinal with relTol 0 is a waste of time, I guess. I would commend out that "p_rghFinal" block. 4) This is a PIMPLE based solver, right? You use "nOuterCorrectors 1" which basically means, that you don't run PIMPLE but PISO. But PISO needs a Courant number of less than 1, which is already violated in the 3rd or 4th time step. Thus, you need to reduce the time step or increase the numer of outer (PIMPLE-)iterations per time step. If you do the second, you should set turbOnFinalIterOnly to "no" and also use some safer relaxation factors for the pressure (such as p 0.3) for the beginning. Try to set nOuterCorrectors 15 or so and see if that runs stable.
__________________
The skeleton ran out of shampoo in the shower. |
|
October 12, 2015, 08:51 |
|
#13 | |
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 10 |
Quote:
3) relTol 0 on p_rghFinal will be removed! 4) I'm using 'interFoam'solver and this solver may be based on PIMPLE algorithm.. I missed that the 'nOuterCorrector 1' means calculation is running PISO algorithm.. Thanks for your kind advice Those 4 advice will be adopted to my case and I'll update results! |
||
October 13, 2015, 04:37 |
|
#14 |
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 10 |
Well,
every advices applied to new case! 1) uncorrected laplacian scheme, 2) Gauss upwind scheme for all fvSchemes 3) relTol 0 was removed 4) nOuterCorrectors 15, turbOnFinalIterOnly no Now, I can see that bounding k is getting bigger and bigger Finally, the calculation blow up and openfoam do Iteration 1000 suddenly in final pimple iteration (Iteration 15)... Here is my log file and fvSolution & fvSchemes... * When I run simulation with turbOnFinalIterOnly yes the volume fraction went above 1.. Can someone explain how turbOnFinalIterOnly affect the pimple iteration or recommend some paper to study? |
|
October 13, 2015, 04:50 |
|
#15 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
Jason, I don't know the solver you use and also don't know what it solves for
But: Is there any differential equation for "alpha" that is solved? Like a transport equation? You need to set an under-relaxation factor for PIMPLE for all the values (such as k, epsilon, p, alpha), otherwise this will probably be very unstable. Please try that. For debugging: You can have a look at the residuals "before" and "after" setting the new under-relaxation factor in the log file. If they change, you set the right value.
__________________
The skeleton ran out of shampoo in the shower. |
|
October 15, 2015, 23:44 |
|
#16 |
Senior Member
Elham
Join Date: Oct 2009
Posts: 184
Rep Power: 16 |
Hi,
I had a very awfull number of iteration for p-rgh, around 190, and after changing relTol from 0 to 0.001 it is great, around 10. Thanks for your advice. |
|
October 16, 2015, 02:17 |
|
#17 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
Great, but does it converge now?
__________________
The skeleton ran out of shampoo in the shower. |
|
October 16, 2015, 02:52 |
|
#18 |
Senior Member
Elham
Join Date: Oct 2009
Posts: 184
Rep Power: 16 |
Unfortunately, I didn't pay attention to the second attempt for solving p-rgh which is still have high No iteration.
MULES: Solving for alpha.water MULES: Solving for alpha.water MULES: Solving for alpha.water Phase-1 volume fraction = 2.111971e-05 Min(alpha1) = 0 Max(alpha1) = 0.9974017 GAMG: Solving for p_rgh, Initial residual = 0.05853901, Final residual = 5.498377e-05, No Iterations 6 time step continuity errors : sum local = 3.274181e-09, global = 1.346159e-14, cumulative = -6.08748e-09 GAMG: Solving for p_rgh, Initial residual = 0.0001254836, Final residual = 9.72051e-07, No Iterations 80 time step continuity errors : sum local = 5.814538e-11, global = 5.793274e-17, cumulative = -6.08748e-09 ExecutionTime = 80707.64 s ClockTime = 81027 s |
|
October 16, 2015, 03:17 |
|
#19 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
You could try a different smoother for the GAMG.
Code:
p { solver GAMG; tolerance 1e-12; relTol 0.1; smoother DICGaussSeidel; nPreSweeps 0; nPostSweeps 1; nFinestSweeps 2; scaleCorrection true; directSolveCoarsestLevel false; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 500; mergeLevels 1; maxIter 100; }
__________________
The skeleton ran out of shampoo in the shower. Last edited by RodriguezFatz; October 16, 2015 at 04:52. |
|
October 13, 2015, 05:08 |
|
#20 |
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 |
Edit: I just made some pictures of your residuals over iteration / time. This looks ugly. I will post the picture.
__________________
The skeleton ran out of shampoo in the shower. |
|
Tags |
convergence, diverge, interfoam |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
a problem with convergence in buoyantSimpleFoam | skuznet | OpenFOAM Running, Solving & CFD | 6 | November 15, 2017 12:12 |
High Courant Number @ icoFoam | Artex85 | OpenFOAM Running, Solving & CFD | 11 | February 16, 2017 13:40 |
Extrusion with OpenFoam problem No. Iterations 0 | Lord Kelvin | OpenFOAM Running, Solving & CFD | 8 | March 28, 2016 11:08 |
should Courant number always be kept below 1? | wc34071209 | OpenFOAM Running, Solving & CFD | 16 | March 9, 2014 19:31 |
rhoSimplecFoam Mach0.8 no pressure values | CFDnewbie147 | OpenFOAM Running, Solving & CFD | 16 | November 23, 2013 05:58 |