
[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: 9 
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 = 2.10029456432146e06, Final residual = 0.0004465071153368, No Iterations 1000 Phase1 volume fraction = 0.626758885470715 Min(alpha1) = 0 Max(alpha1) = 2.51427683470041 MULES: Correcting alpha.water MULES: Correcting alpha.water MULES: Correcting alpha.water Phase1 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 = 3.65937145748082e07, global = 1.53699517734662e08, cumulative = 1.53784861589855e08 GAMG: Solving for p_rgh, Initial residual = 0.0312962317006745, Final residual = 1.39933880273081e05, No Iterations 5 GAMG: Solving for p_rgh, Initial residual = 0.00996448307785306, Final residual = 7.62790351177124e06, No Iterations 5 time step continuity errors : sum local = 3.52922607711308e08, global = 7.58057755027101e10, cumulative = 1.61365439140126e08 GAMG: Solving for p_rgh, Initial residual = 0.00468422248968285, Final residual = 4.66016854885601e06, No Iterations 5 GAMG: Solving for p_rgh, Initial residual = 0.00252317454590901, Final residual = 3.49969247968792e08, No Iterations 12 time step continuity errors : sum local = 1.63507334863481e10, global = 2.95406036297376e12, cumulative = 1.61394979743756e08 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: 25 
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:
"(UkepsilonomegaUFinalkFinalepsilonFinalomegaFinal)" { solver PBiCG; preconditioner DILU; tolerance 1e12; relTol 1.0e2; maxIter 100; };
__________________
The skeleton ran out of shampoo in the shower. 

October 8, 2015, 09:22 

#3 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 25 
Just additionally, this is probably not the reason for your problems but you should always start a case with the uncorrected laplacian scheme, which is numerically more stable.
Code:
laplacianSchemes { default Gauss linear uncorrected; }
__________________
The skeleton ran out of shampoo in the shower. 

October 8, 2015, 10:07 

#4 
Senior Member
Jan
Join Date: Jul 2009
Location: Hamburg
Posts: 119
Rep Power: 18 
There is no reason why an unstructured tet mesh should work better than a structured mesh. I would never prever a tet mesh for free surface flows. Can you plot some screenshots of your mesh and from your initialized solution (especially alpha field)?


October 9, 2015, 12:58 

#5 
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 9 
Thanks for your kind comment. I'll try other solver that you recommended and then update the result. Thank you!


October 9, 2015, 13:00 

#6 
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 9 
Thank you JNSN! I'll update screenshot of mesh later.


October 10, 2015, 09:47 
Thanks! Philipp

#7  
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 9 
Quote:
I tried to use PBiCG solver you suggested Now the K, epsilon iterations become stable Code:
DILUPBiCG: Solving for alpha.water, Initial residual = 9.41257114753943e07, Final residual = 6.69250718355886e11, No Iterations 1 Phase1 volume fraction = 0.626760378142215 Min(alpha1) = 1.16185071173307e06 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 Phase1 volume fraction = 0.626760378142315 Min(alpha1) = 1.16185071173307e06 Max(alpha1) = 1.00150901821138 GAMG: Solving for p_rgh, Initial residual = 0.000268113771479435, Final residual = 1.31199231523444e07, No Iterations 5 GAMG: Solving for p_rgh, Initial residual = 8.9469043939113e05, Final residual = 8.44752800100194e08, No Iterations 5 time step continuity errors : sum local = 1.15163397615092e11, global = 1.29175373620592e12, cumulative = 1.64869290559949e06 GAMG: Solving for p_rgh, Initial residual = 4.07512657567795e05, Final residual = 3.94730642661602e08, No Iterations 6 GAMG: Solving for p_rgh, Initial residual = 3.7833103278026e05, Final residual = 3.70998267918502e08, No Iterations 5 time step continuity errors : sum local = 5.07003233184369e12, global = 7.53555301266291e13, cumulative = 1.64869215204419e06 GAMG: Solving for p_rgh, Initial residual = 1.44866320494826e05, Final residual = 3.79502063541261e08, No Iterations 4 GAMG: Solving for p_rgh, Initial residual = 1.19072340126574e05, Final residual = 4.81493222880152e08, No Iterations 3 time step continuity errors : sum local = 6.55465097078055e12, global = 4.41939941264471e13, cumulative = 1.64869259398413e06 DILUPBiCG: Solving for epsilon, Initial residual = 0.000317455367614486, Final residual = 3.20877793792615e07, No Iterations 2 DILUPBiCG: Solving for k, Initial residual = 8.09326775207824e09, Final residual = 8.09326775207824e09, 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 10, 2015, 09:51 
Here is the picture

#8  
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 9 
Quote:
I attached alpha field screenshot. I'm not sure this picture is that you wanted to see... Well, by the way, I had same trouble(too many iterations for k, epsilon..) when I used Hex mesh(Structured grid)... Thanks! 

October 12, 2015, 07:14 

#9 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 25 
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 

#10 
Senior Member
Jan
Join Date: Jul 2009
Location: Hamburg
Posts: 119
Rep Power: 18 
Jason, I can't see the screenshots. Can you upload again?


October 12, 2015, 07:53 

#11  
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 9 
Quote:
Actually, I stopped the calculation because the residual is getting weird.. Thanks, tigger 

October 12, 2015, 07:54 

#12 
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 9 
Oops, I forgot to attach screenshot
Here it is Thanks, tigger 

October 12, 2015, 07:56 

#13 
Senior Member
Jan
Join Date: Jul 2009
Location: Hamburg
Posts: 119
Rep Power: 18 
ok, can you do one more with mesh grid on?


October 12, 2015, 08:04 

#14 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 25 
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 

#15 
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 9 
Here it is


October 12, 2015, 08:25 

#16 
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 9 


October 12, 2015, 08:34 

#17 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 25 
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 

#18  
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 9 
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 

#19 
New Member
Jason
Join Date: May 2015
Posts: 14
Rep Power: 9 
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 

#20 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 25 
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 underrelaxation 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 underrelaxation factor in the log file. If they change, you set the right value.
__________________
The skeleton ran out of shampoo in the shower. 

Tags 
convergence, diverge, interfoam 
Thread Tools  Search this Thread 
Display Modes  


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 