CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   Applying turbulence model on laminar flow (http://www.cfd-online.com/Forums/main/75304-applying-turbulence-model-laminar-flow.html)

 mannobot April 21, 2010 12:31

Applying turbulence model on laminar flow

Hi,

what happens when I do apply a turbulence model on a laminar flow field?

 agd April 21, 2010 14:28

You get a meaningless result.

 Jade M April 21, 2010 14:30

I wondered the very same thing myself.

I guess the basic answer is that turbulence models can introduce things that are non-physical 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.cfd-online.com/Forums/cfx/73871-cfx-treatment-laminar-turbulent-flows-new-post.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 k-omega, SST, BSL Reynolds Stress, BSL EARSM and BSL agreed well. k-epsilon, SSG Reynolds Stress and k-epsilon 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.

 agd April 21, 2010 15:50

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.

 Jade M April 21, 2010 15:58

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 constant-area duct for which the flow is turbulent, then through a series of fins for which the flow is laminar, and then through another constant-area 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.

 mannobot April 22, 2010 03:46

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

 DoHander April 22, 2010 08:31

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 - Transition-Flow-Occurrence 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 A-B laminar B-C transitional C-D turbulent and say E-F laminar again (if the flow will re-laminarize).

Do

 DoHander April 22, 2010 08:33

Also in Fluent 12 you have now two transition models, which theoretically will detect automatically the laminar/turbulent regions from your flow.

Do

 Jade M April 22, 2010 08:35

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!

 Jade M April 22, 2010 08:42

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 epsilon-based models were way off and all results produced by omega-based 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!

 agd April 22, 2010 12:27

I don't know anything about CFX (I use in-house 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.

 Jade M April 22, 2010 12:28

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 k-epsilon 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 k-epsilon, 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 constant-area 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 constant-area 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 k-epsilon is not suited for this problem?

I'm also curious as to which situations the k-epsilon model might give very good results. Perhaps the k-epsilon model is not really needed since SST and other omega-based models seem to address the deficiencies of epsilon-based models without any disadvantages?

I'd very much appreciate your feedback. Thanks so much for any comments.

 agd April 22, 2010 14:46

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 k-eps model, the points you make are all valid, and to one degree or another show up in all RANS-type models. I typically use the SST model and have found it to work well for attached and separated flows. The hybrid models that incorporate LES-like 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 grid-scale eddy behavior).

 Jade M April 22, 2010 14:55

Thanks so much agd.

Good to know the disadvantages of k-epsilon. 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?

 mannobot April 23, 2010 04:35

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

 DoHander April 23, 2010 08:41

@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

 agd April 23, 2010 09:06

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.

 Jade M April 23, 2010 09:46

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.

 mannobot April 23, 2010 10:01

@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

 agd April 23, 2010 11:51

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 02:29.