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

About kEpsilon turbulence model

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 6, 2006, 17:17
Default Hi, this problem bothered me f
  #1
New Member
 
Simon Zhang
Join Date: Mar 2009
Posts: 18
Rep Power: 8
osimonsimon is on a distinguished road
Hi, this problem bothered me for a while and I really couldn't find a way to figure it out. Basically I am running a 3D simulation using simpleFoam. The model is like a room with multiply inlets (nine) and oulets (two). All of them are velocity inlets(outlets), i.e. the velocity is known at all these boundaries. I followed the tutorial to calculate the initial k and Epsilon at time "0" for all the boundaries. And also set the value for the internal field by guessing a number within the range (between min and max of k(or Epsilon)). I found that the convergence is GREATLY depended on the initial guess of k and Epsilon for the internalField and very sensitive to them. The flow field is also stongly depended on the initial guess of k and epsilon. I've tried a lot of combinations and still have problems getting expected convergence.

Does anyone have any suggestions to this kind of problem? This problem holds me up for quite a while and it is killing me... Please help! Thank you a bunch!
osimonsimon is offline   Reply With Quote

Old   November 7, 2006, 06:05
Default Well I am surprised you get an
  #2
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Well I am surprised you get any convergance at all seeing as you have specified the velocity on all boundaries. The system is over-specified. Try making (at least one of) the outlet velocities zeroGradient.

At convergance simpleFoam results should be more-or-less independant of the starting conditions.
eugene is offline   Reply With Quote

Old   November 7, 2006, 09:27
Default Thanks Eugene. Sorry I forgot
  #3
New Member
 
Simon Zhang
Join Date: Mar 2009
Posts: 18
Rep Power: 8
osimonsimon is on a distinguished road
Thanks Eugene. Sorry I forgot to mention that there is an outlet that is velocity zeroGradient and zero pressure.
osimonsimon is offline   Reply With Quote

Old   November 7, 2006, 12:24
Default As long as your boundary condi
  #4
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
As long as your boundary conditions are the same, the flow should converge to an identical solution independent from the initial conditions. Of course convegence will be affected by the initial conditions, this is normal.

Specifiying a fixed value outlet velocity is not a very good idea even if you have zeroGradient on one of the oulet boundaries. What we really need is some kind of flow split boundary if the mean outlet mass flow distribution is known. This is doable, but has not been implemented to date.

Also, make sure your k and epsilon are zero gradient on the fixed value outflow boundaries. Check that you have no inflow at your zero-gradient outflow boundary, this tends to cause a lot of stability problems. Typically you should run potentialFlow to get a reasonable initial guess for velocity, and use the inletOutlet boundary with inletValue set to (0 0 0) to prevent inflow.

We are working on a more sensible way to specify the initial conditions, but for the time being you have to provide it. For turbulence properties I typically use the values calculated from turb intensity, velocity and lengthscale at the inlet to populate the internal domain.
eugene is offline   Reply With Quote

Old   November 8, 2006, 02:48
Default I can't promise that it will s
  #5
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
I can't promise that it will solve your initialization problems, but you could try using this setKepsilon.tar.gz utility for setting tke and epsilon based on turbulent intensity and length scale. The initial epsilon values seem to cause most of the stability problems.
olesen is offline   Reply With Quote

Old   November 8, 2006, 11:58
Default Thanks Eugene and Thanks Mark!
  #6
New Member
 
Simon Zhang
Join Date: Mar 2009
Posts: 18
Rep Power: 8
osimonsimon is on a distinguished road
Thanks Eugene and Thanks Mark! I really appreciate your help!!

Eugene, thanks for your advise. They do improve the convergence but not much. I changed the k and epsilon to zero gradient on the fixed value outlow boundaries. And no inflow was observed. I was using the same method calculating the initial value of k and epsilon at inlets. For the internal Field, I just pick one a value from those on the inlets. Now I just change these two values (initial valuce of k and epsilon for internal field) and the convergence varies a lot. Some times it getting singularity solutions; sometimes it blows up (continuity); sometimes it converges to 1e-6 for all the variables, but the k is around 3~12 and epsilon is around 20~30, something like that...I am really confused about this. Any comments about these?

Mark, Thanks for sharing the utility. But it seems I could not download the file. Could you please check the link?

Again, thanks very much for you guys' help!
osimonsimon is offline   Reply With Quote

Old   November 9, 2006, 02:48
Default I just downloaded the utility
  #7
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
I just downloaded the utility from the server without a hitch, but the downloaded filenames are indeed a bit odd. In this case it is 'setKepsilon_tar-3364.unk', but the file command reveals that it really is a gzip'd tar file. Just rename and you should be fine.
olesen is offline   Reply With Quote

Old   November 9, 2006, 10:43
Default Yep, you are right. It works.
  #8
New Member
 
Simon Zhang
Join Date: Mar 2009
Posts: 18
Rep Power: 8
osimonsimon is on a distinguished road
Yep, you are right. It works. I will try this out. THanks a lot, Mark!
osimonsimon is offline   Reply With Quote

Old   April 23, 2008, 19:05
Default Does anyone have a good source
  #9
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 546
Rep Power: 18
chegdan will become famous soon enough
Does anyone have a good source explaining what the inlet conditions for k and epsilon should be or how they should be calculated? I'm running a case in simpleFoam of a turbulent reactor (using the k-epsilon model) and I have no idea what the inlet value of k and epsilon should be. Thoughts?
__________________
Dan

Find me on twitter @dancombest and LinkedIn
chegdan is offline   Reply With Quote

Old   April 23, 2008, 19:44
Default Hey, Try the Fluent online
  #10
New Member
 
Ryan Middleton
Join Date: Mar 2009
Posts: 17
Rep Power: 8
ryan_m is on a distinguished road
Hey,

Try the Fluent online user manual:

http://jullio.pe.kr/fluent6.1/help/h....htm#ke-params

It got some pretty simple equations to use for determining turbulent inlet conditions.

Cheers
ryan_m is offline   Reply With Quote

Old   April 24, 2008, 02:52
Default That's where the two following
  #11
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
That's where the two following bc types should be useful:

Calculate turbulent kinetic energy from the intensity provided as a fraction of the mean velocity.
Example of the boundary condition specification:
inlet
{
type turbulentIntensityKineticEnergyInlet;
intensity 0.05; // 5% turbulence
value uniform 1; // placeholder
}

Calculate epsilon via the mixing length [m].
Example of the boundary condition specification:
inlet
{
type turbulentMixingLengthDissipationRateInlet;
mixingLength 0.005; // 5 mm
value uniform 200; // placeholder
}

... assuming, of course, that you have an idea of which intensity and length scales might be relevant for your case.
olesen 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
KEpsilon model k_oldTime not working harly OpenFOAM Running, Solving & CFD 2 December 10, 2008 14:13
Modify kEpsilon model harly OpenFOAM 5 December 3, 2008 18:43
mshaADD A NEW RELATION TO kepsilon MODEL msha OpenFOAM Running, Solving & CFD 3 January 6, 2008 08:06
msha ADD A NEW RELATION TO kepsilon MODEL msha OpenFOAM 0 December 30, 2007 10:30
Adjusting kepsilon model braennstroem OpenFOAM Running, Solving & CFD 2 April 12, 2005 09:52


All times are GMT -4. The time now is 21:56.