# Strange Nut behaviour with K-OmegaSST

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 March 22, 2011, 15:44 Strange Nut behaviour with K-OmegaSST #1 New Member   Join Date: Mar 2011 Posts: 17 Rep Power: 7 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?

 March 22, 2011, 17:04 #2 Senior Member   Felix L. Join Date: Feb 2010 Location: Hamburg Posts: 165 Rep Power: 10 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.

 March 22, 2011, 17:49 #3 New Member   Join Date: Mar 2011 Posts: 17 Rep Power: 7 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

 March 23, 2011, 14:12 #4 Senior Member   Felix L. Join Date: Feb 2010 Location: Hamburg Posts: 165 Rep Power: 10 What about nut, what are you using for that?

 March 23, 2011, 14:35 #5 New Member   Join Date: Mar 2011 Posts: 17 Rep Power: 7 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

 March 23, 2011, 15:46 #6 Senior Member   Felix L. Join Date: Feb 2010 Location: Hamburg Posts: 165 Rep Power: 10 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.

 March 23, 2011, 15:54 #7 New Member   Join Date: Mar 2011 Posts: 17 Rep Power: 7 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.

 March 31, 2011, 15:47 #8 New Member   Join Date: Mar 2011 Posts: 17 Rep Power: 7 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.

 April 3, 2013, 08:48 #9 Member   Malik Join Date: Dec 2012 Location: Austin, USA Posts: 52 Rep Power: 5 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 !

December 25, 2014, 11:57
Spot the error please
#10
Senior Member

Hasan K.J.
Join Date: Dec 2011
Location: Bristol, United Kingdom
Posts: 196
Rep Power: 6
Hey everyone,

Can some one tell me which Nut and K contour plots are wrong below !! for KWSST case.
I have used the same case file but used two different airfoils NACA 0012 and 6512-63
I do not know why there is such a drastic difference between them with Nut and K both have the same BC and inputs.

Quote:
 Originally Posted by FelixL 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.
from this above quote can i conclude that 0012 nut is right !!! anybody any thoughts
If one is wrong can someone tell which one is wrong and what could be causing the error.

Thanks for your replies,
Hasan K.J
Attached Images
 6512-63K.jpg (16.6 KB, 45 views) 6512-63Nut.jpg (15.6 KB, 43 views) 0012K.jpg (15.5 KB, 43 views) 0012Nut.jpg (30.2 KB, 48 views)

Last edited by Alhasan; December 25, 2014 at 14:03.

 January 29, 2015, 12:53 #11 New Member   Join Date: May 2013 Posts: 23 Rep Power: 5 Hello, Do we have update about this observation of k omega SST behaviour ? I am really surprised as well with the complete destruction of turbulence close to the leading edge of a NACA 0009 at 0 incidence angle. The k omega sst model is insensible to the freestream turbulence imposed as inlet. It is acting as whatever the turbulence levels we impose at inlet, the turbulence is artificially destroyed and the NACA profile leading edge "sees" a laminar flow. I have ran 3 test cases, k omega SST, RKE and and k omega. The k omega is performing well, obtaining a 0 turbulence viscosity ratio at the walls adn without this "bump" on the leading edge. The RKE and k omega SST exhibit the "bump" in turbulent viscosity ratio, which seems unphysical to me. Any idea about what is going on ? I have tried to play with the Production Limiter term but it almost does not change the flow features...

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post hani OpenFOAM Running, Solving & CFD 20 March 6, 2013 11:06 Peter85 OpenFOAM Running, Solving & CFD 11 November 18, 2010 02:32 A.Devesa OpenFOAM Running, Solving & CFD 0 April 6, 2010 03:58 ivan_cozza OpenFOAM Running, Solving & CFD 2 February 6, 2010 07:09 segersson OpenFOAM Running, Solving & CFD 0 December 9, 2009 04:57

All times are GMT -4. The time now is 07:49.

 Contact Us - CFD Online - Top