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

Strange Nut behaviour with K-OmegaSST

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

Like Tree1Likes
  • 1 Post By nicolarre

Reply
 
LinkBack Thread Tools Display Modes
Old   March 22, 2011, 15:44
Default Strange Nut behaviour with K-OmegaSST
  #1
New Member
 
Join Date: Mar 2011
Posts: 17
Rep Power: 5
nicolarre is on a distinguished road
Hello,

I was trying out diferent models in a simpleFoam 2-D Ahmed body case.

I ran the same case with both Kepsilon and KomegaSST and got some strange results in NUT in the KomegaSST case.

PIC 1 - Kepsilon result for Nut



PIC 2 - KomegaSST result for Nut


besides the fact that both have very diferent solutions, i noted the strange "bump" at the upper front part of the body.

I thought the solver was doing something wrong with the nut calculator so i used the calculator filter to manually calculate nut with:

nut = k / omega and this is the result

PIC 3 - KomegaSST with nut = k/omega




The "bump" is not there. that means komegaSST was not calculating nut as k/omega, at least not always.

i found on the Wiki ( http://www.cfd-online.com/Wiki/SST_k-omega_model ) that KomegaSST uses a selector in its calculation for nut, choosing the biggest value between a1*omega and S*F2 to calculate nut, like so:

nut = a1*K / Max(a1*omega,S*F2)

i read in this thread (Wrong calculation of nut in the kOmegaSST turbulence model) that there was an error in OPENfoam 1.7.1 with the nut calculation, so i got the fixed version from 1.7.x.


PIC 4 - KomegaSST result for Nut with 1.7.x fix





I assume the "bump" sector is where S*F2 is bigger than a1*omega.

The bump got bigger, since the correction in 1.7.x further reinforces the S*F2 part.

The thing is, i donk know what S*F2 means, nor the reason why its there. It really bugs me because this solution doesnt look right.

The change between k/omega and a1*k/S*F2 is too steep and i fear it may render my solution useless.

Maybe my Y+ is causing trouble, since its pretty horrible

PIC 5 - YPlus fixed



im using the Y+ fix from this thread (http://www.cfd-online.com/Forums/ope...s-1-7-1-a.html)

PIC 6 - YPlus without the fix



Any ideas on why is this happening and how can i avoid it?
nicolarre is offline   Reply With Quote

Old   March 22, 2011, 17:04
Default
  #2
Senior Member
 
Felix L.
Join Date: Feb 2010
Location: Hamburg
Posts: 165
Rep Power: 8
FelixL is on a distinguished road
Hey, nicolarre,


the term max(a1*omega,F2*S) is a stress limiter to improve the model's predictive capabilities especially when shocks play a significant role in the flow. The factor F2 is a switch making sure the stress limiter is only active inside the inner regime of the boundary layer. Outside the boundary layer - where k-Omega-SST uses the k-Epsilon equations - this function's value should be 0 and thus the stress limiter should be inactive, nut is then calculated with nut=k/omega.

If we assume F2 is 1 (inner part of the boundary layer), the stress limiter is very similar to the one in WILCOX' k-Omega turbulence model, the only difference is a constant coefficient (MENTER: 3.23 ; WILCOX: 2.91). If you need further information about what the stress limiter does, please look inside WILCOX' book (Turbulence Modeling for CFD, 3rd Ed.).

In your case... I suspect it's the F2 function causing trouble. Probably it's 1 in the stagnation region in front of your body, even very far away from the wall where you observe that "bump". I observed something very similar when doing simulations on a flat plate with a small leading edge radius, but I didn't really think it strongly affected the results.

Please have a look here about how F2 is calculated, maybe you can calculate it inside paraView. A contour plot of it would give much insight.

There remains an important question: your y+ distribution is really bad, yeah. Are you using wall functions? If so what WFs are you using?
If you're not using any wall functions I wouldn't be surprised about the bad performance of the Menter-SST-Turbulence model with those poorly resolved near wall regions.


Greetings,
Felix.
FelixL is online now   Reply With Quote

Old   March 22, 2011, 17:49
Default
  #3
New Member
 
Join Date: Mar 2011
Posts: 17
Rep Power: 5
nicolarre is on a distinguished road
Felix L, thank you for your reply
Yes, Y+ is horrible. im making a new mesh to fix that

im using the following wall functions on both the floor and the body

Omega:

omegaWallFunction
uniform 0;

K:

kqRWallFunction
uniform 0;

ill try the new mesh and see if the problem is fixed
nicolarre is offline   Reply With Quote

Old   March 23, 2011, 14:12
Default
  #4
Senior Member
 
Felix L.
Join Date: Feb 2010
Location: Hamburg
Posts: 165
Rep Power: 8
FelixL is on a distinguished road
What about nut, what are you using for that?
FelixL is online now   Reply With Quote

Old   March 23, 2011, 14:35
Default
  #5
New Member
 
Join Date: Mar 2011
Posts: 17
Rep Power: 5
nicolarre is on a distinguished road
i dont specify bounding and starting conditions for nut. i let OpenFoam do that by not putting nut in my 0 folder. is this a problem?

i made a new mesh with y+ rangeing from 50 to 200 but got the same result.

in all my cases with KomegaSST, i reach a point where the simulation stops evolving in what seems like a reasonable solution, yet i simplefoam keeps bounding negative values of Omega. idk what causes this nor how to fix it either
nicolarre is offline   Reply With Quote

Old   March 23, 2011, 15:46
Default
  #6
Senior Member
 
Felix L.
Join Date: Feb 2010
Location: Hamburg
Posts: 165
Rep Power: 8
FelixL is on a distinguished road
Uhm, I don't know what happens when you don't specify BCs for nut. OpenFOAM picks a BC maybe or it uses calculated, which would clearly wrong in the case of a HighRe-mesh. I suggest you also specify BCs for nut before running the simulation - it's always better to have full control over everything.

Bounding omega isn't usually a big problem, as long as the negative omega values are close to zero. If you want to get rid of this message, try a different (limited) scheme for div(phi,omega).

If your simulation converges to a reasonable solution (i.e. realistic integral values?), this weird behaviour probably isn't a bug but a feature!

I had a few thoughts about it today and now it sounds okay to me to have low values for turbulent viscosity in stagnation regions. The deceleration of the flow in these regions (-> favorable pressure gradient) tends to dampen the turbulence, lowering the turbulent kinetic energy and thus decreasing nut.
I also doubt if it's okay to compare the results to only one different turbulence model, i.e. kEpsilon. It would be easier to provide a definitive explanation when there are more results with different turbulence models (spalartAllmaras, realizable kEpsilon, ...) available.


Greetings,
Felix.
FelixL is online now   Reply With Quote

Old   March 23, 2011, 15:54
Default
  #7
New Member
 
Join Date: Mar 2011
Posts: 17
Rep Power: 5
nicolarre is on a distinguished road
i've never specified nut BC before. What would be an acceptable field value for nut for air flot @ 40 m/s? i also dont know what would be a usual wall function and value for nut.

I'll run the case on SpalartAllmaras for comparison and maybe a vanilla Komega case

EDIT: i just checked the nut file simpleFoam created in time 0, it automatically sets wall functions for nut


side2
{
type empty;
}
side1
{
type empty;
}
ahmed
{
type nutWallFunction;
Cmu 0.09;
kappa 0.41;
E 9.8;
value uniform 0;
}
inlet
{
type calculated;
value uniform 0;
}
floor
{
type nutWallFunction;
Cmu 0.09;
kappa 0.41;
E 9.8;
value uniform 0;
}
outlet
{
type calculated;
value uniform 0;
}
sky
{
type calculated;
value uniform 0;
}

Last edited by nicolarre; March 23, 2011 at 16:09.
nicolarre is offline   Reply With Quote

Old   March 31, 2011, 15:47
Default
  #8
New Member
 
Join Date: Mar 2011
Posts: 17
Rep Power: 5
nicolarre is on a distinguished road
UPDATE:

i ran some more cases for comparison; Kepsilon, Komega, KomegaSST and SpalartAllmaras on 3 diferent cases.

These are the results.

I still dont understand what's causing that strange behaviour in nut on my KomegaSST cases, but at least its consistent. The low nut "bump" appears in all of them, in roughly the same area.

Ahmed body

(KomegaSSTv2 is KomegaSST with the corrections from version 1.7.x)



Box object

(the KomegaSST, nut =k/omega is exactly that. nut manually calculated as k/omega. Comparing this one with the other KomegaSST nut graph, the only difference between the 2 is that low-nut "bump" at the front)




Semi-circular object




Maybe im misinterpreting what nut is for the KomegaSST model, as i always supposed nut was the property for all models, even its calculation differed from model to model.

What's nut for the KomegaSST model? is it the same that nut for other models? why are the SST solutions so diferent from Ko and Ke when its supposed to be a composite of the two?
JR22 likes this.
nicolarre is offline   Reply With Quote

Old   April 3, 2013, 08:48
Default
  #9
Member
 
Malik
Join Date: Dec 2012
Location: Austin, USA
Posts: 52
Rep Power: 3
malaboss is on a distinguished road
Hi,
I am facing the exact same issue, I really don't understand why KOmegaSST gives values so different from kepsilon for nut.

If I had to choose, I would rather take KomegaSST as nut has to be low were we have stagnation points.

Did you find more info about that ?

Thanks for all !
malaboss 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
Strange behaviour when using LienCubicKE and NonlinearKEShih hani OpenFOAM Running, Solving & CFD 20 March 6, 2013 10:06
Problem with SST-Model - strange behaviour Peter85 OpenFOAM Running, Solving & CFD 11 November 18, 2010 01:32
strange behaviour of GGI in parallel on axis symmetrical case A.Devesa OpenFOAM Running, Solving & CFD 0 April 6, 2010 03:58
fvc::div() strange behaviour ivan_cozza OpenFOAM Running, Solving & CFD 2 February 6, 2010 06:09
Strange behaviour on outlet boundary using LES segersson OpenFOAM Running, Solving & CFD 0 December 9, 2009 03:57


All times are GMT -4. The time now is 11:57.