
[Sponsors] 
What happens with my k and epsilon after a few timesteps 

LinkBack  Thread Tools  Search this Thread  Display Modes 
June 2, 2006, 08:28 
Hello again.
Now I am running

#1 
Member
Marcus Hammar
Join Date: Mar 2009
Posts: 33
Rep Power: 17 
Hello again.
Now I am running a simple 3dmesh with a sphere in a freestream. I am using simpleFoam. During the first few timesteps everything looks good but after a while the magnitudes of "timestep continuity errors", "bounding epsilon" and "bounding k" increases. Anyone knows why? What are typical values of k and epsilon? Is kepsilon the same turbulence model as komega? Thank you! /Marcus 

June 2, 2006, 12:49 
Heya,
kepsilon and komega

#2 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,906
Rep Power: 33 
Heya,
kepsilon and komega (as the name suggests) are two different models. As for your problems, it seems that the discretisation needs tuning: you should not be getting the bouding messages on k and epsilon because if this continues, the solution will blow up. For a better continuity error, try tightening the (relative) pressure tolerance  that's the second number behind p in system/fvSolution (you know where, right?) Enjoy, Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

June 5, 2006, 03:30 
Thank you.
Yes, i know wher

#3 
Member
Marcus Hammar
Join Date: Mar 2009
Posts: 33
Rep Power: 17 
Thank you.
Yes, i know where. /ham 

June 5, 2006, 03:42 
Okey, I tried to tightening th

#4 
Member
Marcus Hammar
Join Date: Mar 2009
Posts: 33
Rep Power: 17 
Okey, I tried to tightening the relative pressure tolerance and yes I got better continuity.
But I guess this is like everything else, a compromise. So when I get better continuity by tightening the pressure tolerance I must be get some negative sideeffects? /marcus 

June 5, 2006, 04:23 
Hi, Im having a similar proble

#5 
Guest
Posts: n/a

Hi, Im having a similar problem where I get all between 50 to 1000 itterations on pressure. when choosing a relative tolerance closer to 0.9 (which is hish) I get most often only one itteration and still low values of continuity. This is what the print out looks like. Is it anything to worry about and should I modify it for a more correct answer?
Time = 0.5 BICCG: Solving for Ux, Initial residual = 0.135647, Final residual = 0.000552089, No Iterations 1 BICCG: Solving for Uy, Initial residual = 0.101647, Final residual = 0.000369054, No Iterations 1 BICCG: Solving for Uz, Initial residual = 0.0413855, Final residual = 0.000171168, No Iterations 1 ICCG: Solving for p, Initial residual = 0.0443585, Final residual = 0.0381298, No Iterations 964 time step continuity errors : sum local = 0.00204006, global = 1.59512e05, cumulative = 0.00112614 Creating alphaEff. BICCG: Solving for T, Initial residual = 0.237459, Final residual = 0.0189455, No Iterations 88 BICCG: Solving for epsilon, Initial residual = 0.0176145, Final residual = 8.30749e11, No Iterations 1 BICCG: Solving for k, Initial residual = 0.147769, Final residual = 0.00053236, No Iterations 1 ExecutionTime = 22.51 s Time = 0.6 BICCG: Solving for Ux, Initial residual = 0.238292, Final residual = 0.000707662, No Iterations 1 BICCG: Solving for Uy, Initial residual = 0.191797, Final residual = 0.000584621, No Iterations 1 BICCG: Solving for Uz, Initial residual = 0.130177, Final residual = 0.000364168, No Iterations 1 ICCG: Solving for p, Initial residual = 0.0319587, Final residual = 0.0173633, No Iterations 1 time step continuity errors : sum local = 0.00206456, global = 0.000150139, cumulative = 0.000976002 Creating alphaEff. BICCG: Solving for T, Initial residual = 0.181806, Final residual = 0.0121908, No Iterations 89 BICCG: Solving for epsilon, Initial residual = 0.040725, Final residual = 8.54144e11, No Iterations 1 BICCG: Solving for k, Initial residual = 0.127848, Final residual = 0.000452815, No Iterations 1 ExecutionTime = 24.83 s Thanks /Erik 

June 5, 2006, 09:35 
But I guess this is like every

#6  
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,906
Rep Power: 33 
Quote:
As for you Erik, try using the AMG solver, this will make it faster. Hrv Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

May 28, 2008, 05:52 
Hi,
I'm also facing the sa

#7 
New Member
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 17 
Hi,
I'm also facing the same kind of problem. I'm working on turbfoam , in my case both epsilon and k are getting bounded and on increasing relative tolerance of either of them they still are bounding and no of iterations is reduced to "1". What can i do to stop it from bounding.........my work has almost come to halt because of this ...please somone reply soon 

June 3, 2008, 05:11 
A common cause of negative k a

#8 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 21 
A common cause of negative k and/or epsilon is an unbounded convection scheme. Switching div(phi,k) and div(phi,epsilon) to "Gauss upwind;" in fvSchemes generally prevents unbounded solutions.
If you are getting negative k and epsilon values despite using upwind for convection, then you probably have some very nasty cells and will have to start looking at reducing your explicit nonorthogonal correction contribution. I must point out though that small negative kepsilon values that cause the bounding routines to trigger are not in themselves problematic. I.e. you can run just fine with bounding removing small negative values of k and epsilon as long as there are no other problems. 

July 15, 2008, 14:12 
Hi,
I am having the same prob

#9 
Senior Member
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 219
Rep Power: 21 
Hi,
I am having the same problem with a negative k that appears to be causing my case to crash. I have tried changing the div(phi,k) to upwind but still get the same problemit crashes after about two iterations. I am using lesInterFoam. Is there maybe something wrong with my boundary specification? I have two pressureInletOutletVelocity boundaries and two fixed value velocity inlets. Any help would be greatly appreciated! 

July 15, 2008, 14:16 
I forgot to also mention that

#10 
Senior Member
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 219
Rep Power: 21 
I forgot to also mention that I am using the locDynOneEqEddy LES model although I have also tried a few others and gotten the same problem.


October 26, 2012, 17:04 

#11 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 
Hello Foamers,
I have a bouding problem in my geometry too, but the bouding value is: Code:
bounding epsilon, min: 1.58155e17 max: 0.0864828 average: 0.0667376 Normally I thought high values are for bounding... Well my pressure calculation is very bad and after 700 timesteps I get 1000 Iterations in the pressure equation. ... I know that problem by using wrong boundary conditions but therefor its not possible to set other BC. 

December 14, 2012, 15:53 

#12 
Member
Aathavan
Join Date: Nov 2012
Posts: 70
Rep Power: 13 
Hi Tobi,
Reply can be late, even though bounding epsilon or k, it can be because of the improper initial values and the schemes which you are using for your div scheme. while using Gauss Linear I was facing this problem, you can fix this problem changing your scheme to upwind for epsilon. Thanks, Aadhavan 

July 7, 2017, 11:18 
bounding K, bounding epsilon

#13  
New Member
rmz
Join Date: May 2017
Location: Paris
Posts: 12
Rep Power: 9 
Hello,
I am also facing problems with k and epsilon (and time step continuity). I am working on a simulation of wind on buildings with a complex Mesh. I am using a RASModel kEspilon with the simpleFoam solver. I am applying ABL conditions (atmospheric boundary layer). the following is the result of simpleFoam: (end of log file) Quote:
bounding epsilon, min: 9.83865826487e+32 max: 1.49104083956e+43 average: 9.07708546183e+36 bounding k, min: 6.88777988968e+34 max: 3.77003683949e+47 average: 1.86101835569e+41 Can anyone help solve this problem? Thank you 

September 10, 2017, 17:33 
bounding epsilon and k (higher values)

#14 
Member
Mehtab
Join Date: Jan 2015
Posts: 41
Rep Power: 11 
Hi,
I am also getting a similar message. I am trying to simulate an open large pool fire with wind effects. I am using fireFoam with ABL. My epsilon and k values are getting higher and higher and epsilon reaching upto 10^18. And courant number drops to 10^10. I tried relaxing pressure in fvSolution to a higher value relTol=0.9 and changed div scheme for k in fvScheme to Gauss upwind. But all in vain. Nothing is changed. Can someone please guide me what might be wrong in this case? Thanks Mehtab 

September 11, 2017, 07:22 

#15 
New Member
rmz
Join Date: May 2017
Location: Paris
Posts: 12
Rep Power: 9 
Hello Mehtab,
In my case, the problem was with the quality of the mesh; the skew faces were causing the k and epsilon to explode. so I worked on fixing my mesh and using schemes that are less sensitive to bad quality mesh. you can check the quality of you mesh using the utility checkMesh. In my case, in order to fix the mesh, i changed the parameters of snappyHexMesh, I used: nSmoothPatch=5 maxBoundarySkewness=3 maxInternalSkewness=2 

September 11, 2017, 08:27 

#16  
Member
Mehtab
Join Date: Jan 2015
Posts: 41
Rep Power: 11 
Hi,
Thanks for the answer. I am not using snappy, I am using blockMesh. My geometry is quite simple with rectangular faces on four sides plus top and ground, and in the centre on the ground, I have fire source. I checked the mesh and quality look acceptable to me. Quote:
Please help me out of this. 

September 11, 2017, 11:04 

#17 
Senior Member
Oskar
Join Date: Nov 2015
Location: Poland
Posts: 184
Rep Power: 10 
Hello.
Your case is really over 200meter in all directions? What were Your relaxation factors? I had similar problem with bounding k and epsilon and relaxation factors solve the problem for me. Did You set relaxation factor for k and epsilon to (for example) 0.05? 

September 16, 2017, 17:22 

#18 
Member
Mehtab
Join Date: Jan 2015
Posts: 41
Rep Power: 11 
Hi,
Yes, my case is really big. I am simulating Montoir 35 m pool fire with wind condition. Yes, I also tried with reducing relaxation factor for k to 0.05 but the result is similar. k and epsilon are shooting high values and causing delta time to be very small and the solution does not forward in time. I am attaching the case files. Please have a look and give any clue what is wrong in the case setup. A part of the log file is attached to accommodate within size limit. Thanks 

August 11, 2019, 22:10 
Gauss Upwind for (k,e,omega) to increase stability

#19 
Member
Chris Harding
Join Date: Dec 2016
Posts: 76
Rep Power: 9 
I assume this is true for all flow geometries.
"Experimentation and previous user experience [2] have shown that the simulated results are insensitive to the discretization scheme used for the convective divergence term in the turbulence equations (for example k, ε or ω). For these equations, use of the upwind discretization scheme ensures stability and does not degrade solution accuracy. This is not the case for the convective divergence term in the momentum equation however, where different discretization schemes can have a significant effect on the results. In particular, the use of upwind discretization in the momentum equation produces significant errors. This is illustrated in detail in Section 5." [1] Anyone disagree and have literature to show why? I am learning. It sure has made my RANS simulation more stable. The user manual says "Gauss Upwind" is considered to be too inaccurate under divergence schemes. As can be seen with the above quote, the authors verify the same for the momentum equation. References: [1] Jones, David A.; Liefvendahl, Mattias; Chapuis, Michael; Widjaja, Ronny; Norrison, Daniel; (2016). RANS Simulations using IpenFOAM Software. URL: https://apps.dtic.mil/dtic/tr/fulltext/u2/1002391.pdf 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Too many VOF subtimesteps problem  wanghong  FLUENT  2  September 11, 2007 02:48 
set number of timesteps in TUI  Gernot  FLUENT  2  May 11, 2006 04:38 
KIVA timesteps  Sasidhar  Main CFD Forum  4  May 8, 2005 08:25 
KIVA Timesteps  Sasidhar  Main CFD Forum  4  April 7, 2005 19:03 
subtimesteps  habib hossainy  FLUENT  0  May 7, 2004 14:26 