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 Tree11Likes
  • 3 Post By hjasak
  • 2 Post By hjasak
  • 4 Post By eugene
  • 1 Post By Aadhavan
  • 1 Post By mehtab

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: 10
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: 1,806
Rep Power: 25
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: 10
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: 10
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: 1,806
Rep Power: 25
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 and aow like 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: 10
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: 14
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, songwukong, aow and 1 others 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: 218
Rep Power: 14
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: 218
Rep Power: 14
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
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,947
Blog Entries: 6
Rep Power: 33
Tobi has a spectacular aura aboutTobi has a spectacular aura about
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 offline   Reply With Quote

Old   December 14, 2012, 16:53
Default
  #12
Member
 
Aathavan
Join Date: Nov 2012
Posts: 70
Rep Power: 7
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

Old   July 7, 2017, 11:18
Exclamation bounding K, bounding epsilon
  #13
rmz
New Member
 
rmz
Join Date: May 2017
Location: Paris
Posts: 12
Rep Power: 2
rmz is on a distinguished road
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:
Time = 1400

--> FOAM Warning :
From function Foam::fv::gaussConvectionScheme<Type>::gaussConvec tionScheme(const Foam::fvMesh&, const surfaceScalarField&, Foam::Istream&) [with Type = Foam::Vector<double>; Foam::surfaceScalarField = Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>]
in file finiteVolume/convectionSchemes/gaussConvectionScheme/gaussConvectionScheme.H at line 124
Reading "/home/ingerop/OpenFOAM/ingerop-4.1/run_Dell/PAP_run/PAP_case_06_30/system/fvSchemes.divSchemes.div(phi,U)" at line 32
Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.
To remove this warning switch off 'warnUnboundedGauss' in "/opt/openfoam4/etc/controlDict"
smoothSolver: Solving for Ux, Initial residual = 0.650123471409, Final residual = 0.000536065354047, No Iterations 7
smoothSolver: Solving for Uy, Initial residual = 0.474402233563, Final residual = 0.000272846612547, No Iterations 7
smoothSolver: Solving for Uz, Initial residual = 0.40187498067, Final residual = 0.000352888200821, No Iterations 7
GAMG: Solving for p, Initial residual = 2.85560731574e-09, Final residual = 3.12227411183e-11, No Iterations 1
GAMG: Solving for p, Initial residual = 1.20231286355e-15, Final residual = 1.20231286355e-15, No Iterations 0
GAMG: Solving for p, Initial residual = 1.20231286355e-15, Final residual = 1.20231286355e-15, No Iterations 0
time step continuity errors : sum local = 6.9024809888e+13, global = 10717.5469682, cumulative = 10682.7233616
smoothSolver: Solving for epsilon, Initial residual = 0.0267368427021, Final residual = 2.3236823785e-05, No Iterations 5
bounding epsilon, min: -9.83865826487e+32 max: 1.49104083956e+43 average: 9.07708546183e+36
smoothSolver: Solving for k, Initial residual = 0.99037016753, Final residual = 0.000816545910787, No Iterations 6
bounding k, min: -2.05212151592e+16 max: 5.16442351974e+35 average: 6.52272709956e+29
ExecutionTime = 29160.12 s ClockTime = 29697 s

Time = 1401

--> FOAM Warning :
From function Foam::fv::gaussConvectionScheme<Type>::gaussConvec tionScheme(const Foam::fvMesh&, const surfaceScalarField&, Foam::Istream&) [with Type = Foam::Vector<double>; Foam::surfaceScalarField = Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>]
in file finiteVolume/convectionSchemes/gaussConvectionScheme/gaussConvectionScheme.H at line 124
Reading "/home/ingerop/OpenFOAM/ingerop-4.1/run_Dell/PAP_run/PAP_case_06_30/system/fvSchemes.divSchemes.div(phi,U)" at line 32
Unbounded 'Gauss' div scheme used in steady-state solver, use 'bounded Gauss' to ensure boundedness.
To remove this warning switch off 'warnUnboundedGauss' in "/opt/openfoam4/etc/controlDict"
smoothSolver: Solving for Ux, Initial residual = 1.73686761346e-09, Final residual = 1.73686761346e-09, No Iterations 0
smoothSolver: Solving for Uy, Initial residual = 8.49670942582e-09, Final residual = 8.49670942582e-09, No Iterations 0
smoothSolver: Solving for Uz, Initial residual = 7.97749175341e-10, Final residual = 7.97749175341e-10, No Iterations 0
GAMG: Solving for p, Initial residual = 3.26294168382e-05, Final residual = 2.04903628538e-08, No Iterations 5
GAMG: Solving for p, Initial residual = 1.80088423459e-12, Final residual = 1.80088423459e-12, No Iterations 0
GAMG: Solving for p, Initial residual = 1.80088423459e-12, Final residual = 1.80088423459e-12, No Iterations 0
time step continuity errors : sum local = 1.92360928162e+41, global = -3.25979779589e+25, cumulative = -3.25979779589e+25
smoothSolver: Solving for epsilon, Initial residual = 2.08398503235e-17, Final residual = 2.08398503235e-17, No Iterations 0
smoothSolver: Solving for k, Initial residual = 8.88019064951e-08, Final residual = 7.39368688472e-11, No Iterations 5
bounding k, min: -6.88777988968e+34 max: 3.77003683949e+47 average: 1.86101835569e+41
ExecutionTime = 29170.4 s ClockTime = 29707 s

SIMPLE solution converged in 1401 iterations

End
so my SIMPLE solution converged but I I have strange bounding k and epsilon:
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
rmz is offline   Reply With Quote

Old   September 10, 2017, 17:33
Default bounding epsilon and k (higher values)
  #14
Member
 
Mehtab
Join Date: Jan 2015
Posts: 41
Rep Power: 4
mehtab is on a distinguished road
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
mehtab is offline   Reply With Quote

Old   September 11, 2017, 07:22
Default
  #15
rmz
New Member
 
rmz
Join Date: May 2017
Location: Paris
Posts: 12
Rep Power: 2
rmz is on a distinguished road
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
rmz is offline   Reply With Quote

Old   September 11, 2017, 08:27
Default
  #16
Member
 
Mehtab
Join Date: Jan 2015
Posts: 41
Rep Power: 4
mehtab is on a distinguished road
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:
Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
points: 644885
faces: 1911936
internal faces: 1889664
cells: 633600
faces per cell: 6
boundary patches: 4
point zones: 0
face zones: 0
cell zones: 0

Overall number of cells of each type:
hexahedra: 633600
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
inlet 2880 2929 ok (non-closed singly connected)
outlet 13536 13685 ok (non-closed singly connected)
sides 2400 2525 ok (non-closed singly connected)
base 3456 3552 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-106.066 -106.066 0) (106.066 106.066 150)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (4.72868e-16 -6.75293e-18 -7.00289e-17) OK.
Max cell openness = 2.66676e-16 OK.
Max aspect ratio = 19.4052 OK.
Minimum face area = 0.0923684. Maximum face area = 44.7697. Face area magnitudes OK.
Min volume = 0.0556316. Max volume = 134.819. Total volume = 6.75e+06. Cell volumes OK.
Mesh non-orthogonality Max: 43.573 average: 13.8074
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.816862 OK.
Coupled point location match (average 0) OK.

Mesh OK.

End
Is there anything to do with LES as I am using LES with one-equation eddy model and cube-root-delta option? I am really stuck at this point, I do not understand the reason behind this absurd nature.

Please help me out of this.
rmz likes this.
mehtab is offline   Reply With Quote

Old   September 11, 2017, 11:04
Default
  #17
Senior Member
 
Oskar
Join Date: Nov 2015
Location: Poland
Posts: 107
Rep Power: 4
sheaker is on a distinguished road
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?
sheaker is offline   Reply With Quote

Old   September 16, 2017, 17:22
Default
  #18
Member
 
Mehtab
Join Date: Jan 2015
Posts: 41
Rep Power: 4
mehtab is on a distinguished road
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
Attached Files
File Type: zip log.zip (192.6 KB, 3 views)
File Type: zip Montoir-trial-onesideface-outlet.zip (85.3 KB, 1 views)
mehtab 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 02:46.