
[Sponsors] 
March 11, 2011, 12:23 
General question: turbulence and laminar models

#1 
New Member
Join Date: Mar 2011
Posts: 1
Rep Power: 0 
Quick question: What happens when you use a turbulent model in a system where the flow is laminar? Apart from computational costs, how would this affect the result? Would the result be exactly the same as using a laminar model?
The reason I ask this is, in my limited time with CFD, I have just modelled systems that have had some turbulence in them. I modelled a system and, as I usually do, turned on the turbulent parameters within the software without really thinking. I ran the analysis, did mesh studies, y+ etc. However, after all this, when I looked at the boundary inlet, and did some 'hand calculations', I realised, in this particular case, the flow entering had a Reynolds number of 2130, which is laminar. The crunch is, do I have to go back and rerun the analysis with a laminar model, or does it not matter? I used a komega model. Cheers! 

March 11, 2011, 20:03 

#2 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 480
Rep Power: 12 
Your Reynolds number is quite small. The use of a turbulence model will have an effect, how much depends on the level of the eddy viscosity compared to your laminar viscosity. If the ratio is greater than 5, definitely expect differences. But, considering your low Reynolds number, it might not be. It is also a function of your incoming turbulence. Best thing to do is plot up your eddy viscosity and see what it looks like. Also, run a sample set of laminar runs and see how they compare to the ones when using a turbulence model.


March 11, 2011, 22:32 

#3  
Senior Member
Raashid Baig
Join Date: Mar 2010
Location: Bangalore, India
Posts: 136
Rep Power: 9 
Quote:
(Someone please correct me if I am wrong here) It's always safe to run a turbulent simulation, because the flow might be laminar at the inlet, but it might turn turbulent after interacting with the geometry. If that is the case I don't think laminar simulation will be able to capture it properly. Can someone elaborate on this topic ? Raashid 

March 11, 2011, 23:02 

#4 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 480
Rep Power: 12 
Because of the small Reynolds number, I am assuming that the flow features are largeish when compared to geometry scales.
Fluentmonkey should say more about what he is modeling to give a better answer. 

March 12, 2011, 07:10 

#5  
Senior Member
Raashid Baig
Join Date: Mar 2010
Location: Bangalore, India
Posts: 136
Rep Power: 9 
Quote:
1. Is there a definite way by which we can say a flow is laminar/turbulent or in transition ? Is it not dependent heavily on the geometry shape and it is more difficult to define weather a flow is laminar or turbulent for bodies with complicated geometry (like flow over a terrain or flow over an oil rig where there is no single fixed reference length). 2. If we know for sure that a flow is turbulent but we run it as a turbulent simulation, will not the artificial numerical turbulence die on it's own ? In other words what are the pits falls of our choice. Thanks in advance to anyone who enlighten me with these doubts. Raashid 

March 14, 2011, 14:40 

#6 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 480
Rep Power: 12 
Truthfully, I'm not sure what the pitfalls of our choices are.
1) yes defining the reference length is challenging. I don't think there is a good answer. That is part of the art. 2) The eddy viscosity doesn't necessarily die out, or at least die out where it should. 

March 15, 2011, 00:43 

#7  
Senior Member
Raashid Baig
Join Date: Mar 2010
Location: Bangalore, India
Posts: 136
Rep Power: 9 
Quote:
Thanks for the reply. I want to ask weather there is a easy way of predicting weather a flow is laminar or turbulent. To determine if a flow is separated or not there is a very easy way of using surface streamlines (or oil flow patterns) in any major CFD postprocessing software. Is there a similar way by which we can determine this ? I have had some past experience in high speed external aerodynamic flow for such problems, laminar to turbulence transition is of relatively lower importance (Since the flow becomes turbulent very easily) than flow separation. But for low speed problems transition occurs much later is is more difficult to predict. So I want to know is there a definitive and easy way of analyzing if the flow is laminar or turbulent. 

March 15, 2011, 16:13 

#8 
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 480
Rep Power: 12 
I usually look at the eddy viscosity since eddy viscosity is created where the turbulence model thinks there is turbulence. Of course the turbulence model could be wrong...
You can also check out the parameters used as variables for the turbulence source model, such as vorticity for the SA model. 

March 15, 2011, 21:18 

#9 
Senior Member

Hi,
Imposing a turbulence model to a laminar scenario usually results in higher dissipation. But, as Martin pointed out, it is best to put it to the test. On the subject, have a look at the poster presentation http://www.cats.rwthaachen.de:8080/...erFDA2009.pdf . The Re 500 scenario is laminar. The simulations conducted with turbulence model show a sharper decrease in centreline velocity.
__________________
 Julien de Charentenay 

March 16, 2011, 06:11 

#10  
New Member
Vic
Join Date: Feb 2011
Posts: 5
Rep Power: 8 
Quote:
Also for some instances, the Re range in a scenario could vary from hundreds to thousands, but as we can only use one model in the calculation, we have to choose the turbulence? Am I right? Victor 

March 17, 2011, 05:06 

#11  
Senior Member
mohammad
Join Date: Dec 2010
Location: Seoul, South korea
Posts: 214
Rep Power: 9 
Quote:
I have a problem with the values of "eddy viscosity" and "laminar viscosity". I run one wind turbine file in CFX and at the end of the output file i got two eddy viscosity values( max. and min.) for each domain. Since the model contains two domains, I have 4 totally different values for eddy viscosity ranging from 8.81E21 to 1.79 e3. Would you please tell me about this problem? Regards, 

March 17, 2011, 14:49 

#12 
Senior Member
Raashid Baig
Join Date: Mar 2010
Location: Bangalore, India
Posts: 136
Rep Power: 9 
Hi,
I will like to take forum's attention to a very similar problem that I faced while trying to simulate wind turbine NREL phase VI simulations. It's a low speed flow problem where the Reynolds numbers are around 1e06 or below. Experimental results are available for the base aerofoil S809 (See the attached images). These experimental oil flow lines show that they have all the problems associated with low speed laminar flows (Laminar separation, bubble formation and turbulent reattachment). But just today I found a paper by Dr Menter  "Predicting 2D Airfoil and 3D Wind Turbine Rotor Performance using a Transition Model for General CFD Codes", R. Langtry, J. Gola and F. Menter, ANSYS CFX, Otterfing, Germany, AIAA20060395 44th AIAA Aerospace Sciences Meeting and Exhibit It uses the SST Transitional model and surprisingly these are the most consistent set of results that I have seen for this set of experiments. The results may not be very accurate but they manage to give consistency and are always around 10% of the experimental values. Please let me know your thoughts on the same and are there any other methods which can give more accurate and consistent results ??????????? 

March 17, 2011, 15:47 

#13  
Senior Member
Martin Hegedus
Join Date: Feb 2011
Posts: 480
Rep Power: 12 
Quote:
The eddy viscosity at the surface will essentially be zero. A little off the surface the nondimensional value can range from 10 to 100. The value increases as Reynolds number goes up and your inlet turbulence value is increased. The value also increases getting closer to trailing edge. In the wake of a blunt body the non dimensional eddy viscosity can get extremely large, such as 1e4 to 1e5. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Is this understanding of turbulence models correct?  3kha  Main CFD Forum  3  January 31, 2011 22:31 
How to determinate turbulence scale in LES (laminar simulation)?  Franciswu21  ANSYS  0  October 22, 2009 12:48 
turbulence model question  Jason Wei  Main CFD Forum  1  May 6, 2003 00:45 
Turbulence models  pop  Main CFD Forum  3  May 31, 2001 00:16 
turbulence modeling questions  llowen  Main CFD Forum  3  September 11, 1998 04:24 