Applying turbulence model on laminar flow
Hi,
what happens when I do apply a turbulence model on a laminar flow field? Thank you for your answers 
You get a meaningless result.

I wondered the very same thing myself.
I guess the basic answer is that turbulence models can introduce things that are nonphysical in the flow if the flow is truly laminar. I was hoping that the "safe" thing to do is run turbulent so capture all effects (laminar or turbulent). I am by no means an expert in turbulence but I am trying to learn as fast as I can. Please take my comments with a grain of salt. ;)
There are some useful comments from a much more knowledgable person at http://www.cfdonline.com/Forums/cfx/73871cfxtreatmentlaminarturbulentflowsnewpost.html I did recently perform an analysis on a problem which may have had some turbulence in two sections of the flow but was laminar in another section. Running laminar agreed well with correlations. I also ran several turbulence models in CFX and komega, SST, BSL Reynolds Stress, BSL EARSM and BSL agreed well. kepsilon, SSG Reynolds Stress and kepsilon EARSM were way off. This is just my experience with one particular problem. I have not yet figured out how to generalize what I've learned. 
The only meaningful generalization that I have ever developed is that CFD is still essentially binary when it comes to transitional flows  it really only works well if the flow is laminar or turbulent. Some turbulence models have "tripping functions" that can be used, but these typically have to be calibrated for a given problem to get the best results. There are also some transition models (CFX supposedly has a decent one developed by Menter), but the jury is still out on general applicability (last I had heard). So you just have to apply CFD with a great deal of prudence when you are in the transitional regime.

Question for agd
Very interesting.
I have a slightly different but related question that I think you might be shed some light on. What would you recommend if the flow was laminar in over some of the domain and turbulent over some of the domain? An ANSYS FLUENT consultant tells me that one can turn on and off turbulence in different domains if using SST. I did not see where that option existed in CFX. Also this seems that it could become complicated very quickly. Would this involve defining several different domains? In my case, the flow goes through a constantarea duct for which the flow is turbulent, then through a series of fins for which the flow is laminar, and then through another constantarea duct for which the flow is turbulent. I believe the flow is slow enough that there should not be significant leading and trailing edge effects in the finned section. However, the results seem to indicate that there is an adverse pressure gradient which might indicate eddies? Thanks so very much for any thoughts on this. 
Hi,
that is what I thought. But if I am not able to clearly detect the transition point I won't be able to apply different conditions on my model. My problem is that I am not sure wether or not turbulence appears. I am dealing with impingement at very low velocities but I think that after the jet gets deflected and accelerated there might be turbulent effects. So you would recommend to calculate laminar? Kind regards 
Hello,
you can obtain a fair approximation for the turbulent/laminar regions in a flow by doing an entirely laminar unsteady calculation and recording the skin friction history, see this for e.g.: Silisteanu, P., Botez, R  TransitionFlowOccurrence Estimation: A New Method, Journal of Aircraft, Vol. 47, No. 2, March–April 2010 The procedure works but the calculation seems to use a lot of processor resources, however you can (theoretically) detect where the flow became turbulent and if this remains turbulent or not on the remaining of the domain. For example if you have the points A,B,C,D,E,F on a wall surface you could have AB laminar BC transitional CD turbulent and say EF laminar again (if the flow will relaminarize). Do 
Also in Fluent 12 you have now two transition models, which theoretically will detect automatically the laminar/turbulent regions from your flow.
Do 
mannobot,
These are good questions. I think DoHander's suggestion is very helpful. For whatever it's worth, I'll chip in a couple of more comments. If you have the time and computational resources, you might try running different models and see what you get. This is essentially what I did and found agreement between several of the different models, which also agreed with my guestimates based on correlation. Do you have any problem that you can benchmark against? This may be helpful in indentifying whether the solution is reasonable. I would be very interested in what you learn. Take care and good luck! 
Another Question for agd
Hi agd and everyone,
For my problem with the finned section, I ran all the RANS models available in CFX. All results produced by epsilonbased models were way off and all results produced by omegabased models were about the same and correct. I say correct based on agreement with correlations. Do you know why this might be? Thank you so very much for any thoughts. I've been working hard to try to figure this out so your advice would be greatly appreciated! 
I don't know anything about CFX (I use inhouse tools for CFD), so I can't really contribute a lot to your search other than consider the usual suspects  y+ spacing, wall function behavior if you're using wall functions, applicability of the RANS or URANS models for the flow you're modeling, etc.

Thanks so much agd!
I was thinking further. I think my question is more fundamental rather than necessarily CFX related although I'm fairly new to turbulence and CFX so I could be wrong. I say this because I belive I have satisfied the y+ criteria and I believe I have a good mesh. So, I think that the kepsilon model is fundamentally not suited for my problem, but I am trying to figure out why. I have been researching and trying to understand the difference RANS models as fast as I can but I'm probably still lacking greatly in my understanding. I quote a few statements that I found about kepsilon, which are "Widely used despite the known limitations of the model," "Performs poorly for complex flows involving severe pressure gradient, separation, strong streamline curvature," "Valid for fully turbulent flows only," and "Most disturbing weakness is lack of sensitivity to adverse pressure gradients." Are these statements true? In my case, the flow goes through a constantarea duct for which the flow is turbulent, then through a series of fins (several transverse to the flow, and multiple rows in the flow direction) for which the flow is laminar, and then through another constantarea duct for which the flow is turbulent. In the trailing edge regions, there are adverse pressure gradients and there seem to be stagnation regions. Would this be the reason that kepsilon is not suited for this problem? I'm also curious as to which situations the kepsilon model might give very good results. Perhaps the kepsilon model is not really needed since SST and other omegabased models seem to address the deficiencies of epsilonbased models without any disadvantages? I'd very much appreciate your feedback. Thanks so much for any comments. 
One question  you say that the flow moves through a duct where the flow is turbulent and then into a region with some fins where the flow is then laminar. What is driving the relaminarization of the flow?
As far as limitations of the keps model, the points you make are all valid, and to one degree or another show up in all RANStype models. I typically use the SST model and have found it to work well for attached and separated flows. The hybrid models that incorporate LESlike features also work well, although they typically require a little more attention to the meshing (they like relatively uniform meshes in regions where the grid is expected to capture the gridscale eddy behavior). 
Thanks so much agd.
Good to know the disadvantages of kepsilon. It does not sound like there are many advantages? Good point about the relaminarization. I guess that I'm making this statement based on the Reynolds number. From a mathematical point of view, since the fin walls are thin, the velocity is roughly the same throughout the flow but the characteristic dimension decreases in the finned section thereby decreasing Re. Am I totally not making sense? I think you may have hit on something. The streamlines are totally smooth. Do all turbulent flows have eddies? Am I confusing eddies with vorticity? Perhaps this is a laminar flow with separation. Would there be any indicator from looking at the streamlines? 
Hi,
as far as I know you cant decide wether or not a flow field includes turbulence by looking at the streamlines given by CFD. The RANS models do just add terms like additional viscosity. The other point is that it is not possible to just take Re into account to decide about the behaviour of the flow field. To discuss the advantages of kappa epsilon compared to SST models: My experience is that kappa epsilon is more forgiving. I used the realizable kappa epsilon model with enhanced wall treatment which gave me good results (impinging jets:transition zones) under reasonable effort. If you want to study further there is a very nice book WILCOX, D.C.. Turbulence Modelling for CFD, DCW Industries, California,. USA, 1994. @DoHander Assuming I was able to detect those regions, how would I switch turbulence model on and off within FLUENT? Regards 
@mannobot
I see two solutions if you know the regions where your flow is turbulent: 1. Geometrically split the calculation domain in more regions, you can do this in Gambit or in your mesh generator or even in Fluent. Say your domain is a rectangle and you know that after some point on the South side (which is a wall) you have turbulent flow, then simply draw a vertical line on the entire domain and split the mesh in two regions. In Fluent enable a turbulence model, after that you will be able from the Boundary Conditions panel to pick a domain and tell Fluent this is a laminar region. This is the approach used in the above mentioned article. 2. Use a UDF to delimit a certain spatial domain in which you can cancel the turbulent viscosity. This method is potentially more flexible then 1, but harder to implement. Do 
I would be very surprised if the flow relaminarizes  you are carrying turbulence into the fluid from the upstream, and the Re of the fin sections is going to play a significantly reduced role in indicating whether the flow is turbulent or not. The primary mechanism for transition will not be the classic small disturbance growth, but more likely some type of bypass transition. Realistically, I would assume that if the upstream flow is turbulent, then the downstream flow will also be turbulent, based on what I understand of your situation.

Very interesting. Thanks everyone for your thoughtful input. agd, well said. I think you hit the nail on the head. It bothered me the laminar versus turbulent sections. mannobot, good point about using Re to decide on the flow regime.
I guess my question about looking at the streamlines should be clarified  if I use a turbulence model to simulate the problem, would the streamlines show any eddies or any evidence of vorticity if the flow were truly turbulent? Thanks for any further information. This discussion is really clarifying things for me. 
@DoHander
Thanks. I will try to define several domains within ICEM. Do you think I will be able to enable different turbulence modells, each best able to predict the effects in the particular region? Kind regards 
Since the streamlines are only going to reflect the mean velocity field you are not going to get a lot of useful information concerning turbulence. The most straightforward measure is to plot the eddy viscosity as computed by the turbulence model. Vorticity (or another strain measure) could be useful since most turbulence models relate the production to the mean strain rate, but those quantities are strongly dependent on grid quality (which is one big reason why turbulence models are dependent on good grids).

All times are GMT 4. The time now is 07:22. 