CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

What happens with my k and epsilon after a few timesteps

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree7Likes
  • 3 Post By hjasak
  • 1 Post By hjasak
  • 2 Post By eugene
  • 1 Post By Aadhavan

Reply
 
LinkBack Thread Tools Display Modes
Old   June 2, 2006, 08:28
Default Hello again. Now I am running
  #1
ham
Member
 
Marcus Hammar
Join Date: Mar 2009
Posts: 33
Rep Power: 8
ham is on a distinguished road
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 "time-step continuity errors", "bounding epsilon" and "bounding k" increases.

Anyone knows why?
What are typical values of k and epsilon?
Is k-epsilon the same turbulence model as k-omega?

Thank you!

/Marcus
ham is offline   Reply With Quote

Old   June 2, 2006, 12:49
Default Heya, k-epsilon and k-omega
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,753
Rep Power: 21
hjasak will become famous soon enough
Heya,

k-epsilon and k-omega (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
hjasak is offline   Reply With Quote

Old   June 5, 2006, 03:30
Default Thank you. Yes, i know wher
  #3
ham
Member
 
Marcus Hammar
Join Date: Mar 2009
Posts: 33
Rep Power: 8
ham is on a distinguished road
Thank you.

Yes, i know where.

/ham
ham is offline   Reply With Quote

Old   June 5, 2006, 03:42
Default Okey, I tried to tightening th
  #4
ham
Member
 
Marcus Hammar
Join Date: Mar 2009
Posts: 33
Rep Power: 8
ham is on a distinguished road
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
ham is offline   Reply With Quote

Old   June 5, 2006, 04:23
Default Hi, Im having a similar proble
  #5
newbee
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 = -1.59512e-05, 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 = 8.30749e-11, 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 = 8.54144e-11, No Iterations 1
BICCG: Solving for k, Initial residual = 0.127848, Final residual = 0.000452815, No Iterations 1
ExecutionTime = 24.83 s

Thanks
/Erik
  Reply With Quote

Old   June 5, 2006, 09:35
Default But I guess this is like every
  #6
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,753
Rep Power: 21
hjasak will become famous soon enough
Quote:
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?
That is correct: the negative side-effect that you get is the fact that the pressure solver now works harder and as a consequence your simulation time is longer. If you really need bettwr convergence, this cannot be helped....

As for you Erik, try using the AMG solver, this will make it faster.

Hrv


Hrv
songwukong likes this.
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 28, 2008, 05:52
Default Hi, I'm also facing the sa
  #7
New Member
 
Mohd Yousuf
Join Date: Mar 2009
Location: Kharagpur
Posts: 18
Rep Power: 8
yousuf is on a distinguished road
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
yousuf is offline   Reply With Quote

Old   June 3, 2008, 05:11
Default A common cause of negative k a
  #8
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
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 non-orthogonal correction contribution.

I must point out though that small negative k-epsilon 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.
calim_cfd and songwukong like this.
eugene is offline   Reply With Quote

Old   July 15, 2008, 14:12
Default Hi, I am having the same prob
  #9
Senior Member
 
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 191
Rep Power: 10
kwardle is on a distinguished road
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 problem--it 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!
kwardle is offline   Reply With Quote

Old   July 15, 2008, 14:16
Default I forgot to also mention that
  #10
Senior Member
 
Kent Wardle
Join Date: Mar 2009
Location: Illinois, USA
Posts: 191
Rep Power: 10
kwardle is on a distinguished road
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.
kwardle is offline   Reply With Quote

Old   October 26, 2012, 17:04
Default
  #11
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,043
Blog Entries: 4
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hello Foamers,

I have a bouding problem in my geometry too, but the bouding value is:

Code:
bounding epsilon, min: 1.58155e-17 max: 0.0864828 average: 0.0667376
What is causing it?
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.
Tobi is online now   Reply With Quote

Old   December 14, 2012, 16:53
Default
  #12
Member
 
Aathavan
Join Date: Nov 2012
Posts: 69
Rep Power: 4
Aadhavan is on a distinguished road
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
songwukong likes this.
Aadhavan is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Too many VOF sub-timesteps 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
sub-timesteps habib hossainy FLUENT 0 May 7, 2004 14:26


All times are GMT -4. The time now is 04:20.