Two-equation turbulent models: low re airfoils
 

Hello

I am trying to analyse flows past different 2D airfoils at low reynolds numbers (order of 10^4-10^5) and having problems. I am using fluent, but I guess this is not the fluent problem, but rather a general one.

At this reynolds number significant part of the flow over an airfoil is laminar and separation bubbles with transition are formed.

First I run one-equation SA model, which obviously produces turbulent flow over whole airfoil, as there were trips at the leading edge, and generally the drag is overestimated. Here everything is going smooth, but solution is nof of inerest.

At these reynolds numbers you can get a fine mesh without problems, as boundary layer is thik and laminar sublayer can be resolved without wall functions. In my case y+ is order of 1.

Then, to take separation and transition into accound I am trying two equation k-omega and k-omega sst transitional models. Here I am going into the trouble as solution never converges: choise of different discretization schemes, solvers, relaxation parameters, furter refinement of the grid does not help.

Is it a typical problem with two-equation models at this reynolds number?

I was trying to search on the web, but information on application of RANS for these reynolds numbers is quite poor.

If there is somebody who had experience in this kind of simulation:

what solver discretization scheme and relaxation parameters to use?
which initial conditions to set?
which boundary condition for k and omega to set? (I set boundary condition for turbulent quantities based on my x-foil experience: clculated from turbulence intensity of 0.07% and lenght 0.01m at inlet and outlet)

Will be grateful for your help

Truffaldino

I have managed to make to convergence k-omega standard transitional model by iterating standard k-omega until convergence and then running k-omega standard transitional, but results are dissapointing:

the drag coefficient 3.5 times higher than experimental and lift coefficient 10% lower.

Still, k-omega SST diveres whatever I am trying to do

Any help?

Truffaldino

try to first obtain convergence with k-e or k-omega and just then switch to sst. sometimes it might work.

using sst from the beginning of the simulation is really hard in my opinion.

let me know if it help

Why do you expect your solution to converge, i.e. be steady? I assume that is what you mean, i.e. converge to steady state.

I'm not familiar with FLUENT, but I assume you can limit the magnitude of the eddy viscosity. For example, take the solution you have converged with SA and limit the eddy viscosity and see when your solution goes unsteady. If you limit your eddy viscosity to zero you have laminar flow.

Then, compare your eddy viscosity levels from your limited SA model to the eddy viscosity of your other models. I suspect your eddy viscosity from your other models are lower than your fully turbulent solution. Thus, your other transition model solutions are more likely to be unstable.

Thank you for suggestion, swithching

k-omgega ---> k-omega sst ----> k-omega sst transitional

does not help: k-omega goes fine, then k-omega sst still have acceptable residuals, but when finally switching to transitional residuals are oscillating wildly. Perhaps I am using a wrong discretization scheme. Which discretization schemes do you suggest?

No, I mean numeric convergence, i.e. reasonable decrease in resudual. I have tried both stationar and non-stationar solvers: residuals oscillate wildly in kw-sst transitional model. Perhaps indeed the eddy viscosity is too low in k-w sst transitional to de-chaotise the solution. Perhaps I have to set higher turbulence at inlet to see if it will make solution to converge.

simple, second order everything, green-gauss node based, double precision, might require some fiddling with the under-relaxation factors.

can you post a picture of your mesh? with a close up of the trailing edge if possible. just to check that you don't have highly skewed elements due to a sharp trailing edge angle.

also, you might want to check the residuals location in your domain to see if it might influence the solution or not (not sure it might be done in fluent)

might i ask how much the residuals are oscillating? everything or just some values? how many iterations do you use?

I gather what you are saying is that, even for an unsteady problem, your residuals have not converged enough. Since you mentioned separation bubble one of my thoughts is that your k-omega sst transitional model does not have enough eddy viscosity to stabilize the bubble, and the bubble is busting, reforming, bursting, ...

Some additional questions:
1) What is the thickness of your airfoil?
2) What angle of attack are you running?
3) Have you tried running laminar and comparing the solution behavior to your k-omega sst transitional model?
4) Did your k-omega and k-omega sst models converge to a steady or unsteady solution?

Edit: Can you also show us a plot of the eddy viscosity around your airfoil for either the k-omega or k-omega sst models. Thanks.

Trying to predict laminar separation, natural transition and turbulent reattachment using a two-equation turbulence model is a bit optimistic! From my experience two-equation turbulence models like k-eps, k-omega, SST k-omea, ... should only be used when you have fully turbulent boundary layers. The same goes for the SA model. If you want to solve transition you need some form of special transition model or correlation.

Some researchers claim to be able to predict by-pass transition using only two-equation models. Natural transition can never be predicted with a normal two-equation turbulence model! Note the difference between by-pass transtion, caused by diffusion of turbulent energy into the boundary layer from a turbulent free-stream, and natural transition, caused by instabilities in a laminar boundary/shear layer. However, I do not believe that by-pass transition can be reliably predicted using just a two-equation turbulence model. Sometimes you can predict a transitional behaviour, but it does not occur at the correct position and often does not show the correct physical characteristics.

With Fluent most of the two-equation models can not even predict a transitional behaviour. You will get turbulent boundary layers right from the leading edge. The only model implemented in Fluent which I have been able to get any transitional behaviour with is the low-Re Launder-Sharma k-epsilon model.

Yes, I have understood this by looking at result of computation. As far as I undersand it is necessary to introduce user defined intermediency factor or other "artificial" things like that that are uncontrolled and highly unreliable.

Before, I was using x-foil for this kind of analysys and it a way much better than using turbulence models on mesh for airfoil analysys in this range of low reynolds numbers:

My problem is that I want to do an analysys of stepped airfoils, for which x-foil is not suitable, so I decided to try CFD on mesh. To validate the method and get some training I started with conventional airfoils, and it turns out that 2eqn turbulence modelling is not suitable even for them, not to mention stepped airfoils I was going to analyze in prospective!

Perhaps one should use LES in this situation?

Using CFD and normal turbulence models to predict laminar separation/natural transition/turbulent reattachment is VERY difficult and not something that can be done reliably in even very controlled research cases. LES can be used and is used in research. But to do this reliably you need to use some form of transition prediction method or correlation that has been validated for geometries and conditions similar to the one you want to predict. I do not know x-foil, but I assume that it includes some form of correlation to predict this which has been validated on similar cases. I would recommend you to start looking for simple correlations to predict these phenomena and use these correlations to control a user-defined intermittency factor or similar in your CFD code, as you describe. Hence, my recommendation is ad-hoc experimentally validated correlations instead of trying more advanced general CFD methods (LES etc.)

This is sd7037 airfoil (9% thikness) at Re=70000. Sure, there is a separation bubble as you can clearly see from X-foil run shown below: that is why laminar solution never converges, as you have noticed. I will try to upload fluent plots and mesh a bit later.

k-omega converges very well for steady simulation (I set residuals 10^(-6)), k-omega sst oscillates at higher residuals and never reaches 10^(-6).

Thanks Martin,

Seems you are right, see plots for steady simulation form kw (2000 iterations) to kw sst staedy with oscillating residuals (they are also shown). The eddy viscosity is too small. But I am wandering, why then kw-standard converges so good, but overestimates the drag order of magnitude? What turbulence intensity do you sugges at the inlet?

In my case I set intensity 0.07% and turbulence lenght is an airfoil chord.

Thank you a lot! I post a picture of the mes and closeups of LE and TE. Plot of residuals is shown in the previous post.

Truffaldino

The problem here that there is no experimental results for stepped vortex-trapping airfoils, analysys of which is a final goal of thisn work. I wanted to compare performance of this type of airfoils with best conventional ones (and now trying to analyse only conventional ones using CFD code). For conventional airfoils one can establish correlations etc, but these data are of no use in different geometry of vortex-trapping airfoils.

As for x-foil: it uses viscous-nviscid interaction for boundary layer through integral BL methods, transition is predicted by e^n method. Program seems to use some othrer correlations (I am not copletely sure).

Sorry, Truffaldino, I think I mislead you. I gather you plotted eddy viscosity on the actual surface rather than in the flow field. The eddy viscosity on the surface will be very small. Instead, do a 2d contour plot of the eddy viscosity in the region near the airfoil. For example, a region similar to your second grid post, but include more area in front and behind your leading and trailing edge.

In my opinion you also need more grid points at your trailing edge. But use caution with this. If you are using local time stepping to converge the problem, a grid that is too dense at the tailing edge will cause instabilities. I'm not sure if increasing the trailing edge grid density will help your convergence issue, but it will affect your pressure drag.

Your convergence plot is interesting. I'll admit I'm not familiar with Fluent's solution methodology. But, from your plot, it looks like your x and y velocities are converging and your continuity equation is not. (I'm having difficulty matching colors to the variable key) I'll admit I'm not sure what is meant by "continuity" residual. I'm use to seeing variables such as u, v, rho, p, etc. Is continuity a variable? Anyway, if your x and y velocities converge, I would think that the rest would too...

Unfortunately for a 2D airfoil it is easy for your drag to be off. To get a handle on that I would suggest plotting coefficient of friction (cf) and coefficient of pressure (cp) vs x. The coefficient of friction of turbulent flow is about 3 times larger than that for laminar flow. I think. Don't hold me to that. Also, unsteady flow on the back side will probably give you a higher pressure drag than fully attached flow modeled by your turbulence model. What I'm trying to say is that the eddy viscosity from the fully turbulent flow on the back side of the airfoil will dampen, and probably kill, the unsteady flow features thus reducing the pressure drag. Therefore, on on hand, laminar flow gives a higher drag (as compared to RANS) due to unsteadiness on the backside and turbulent flow gives higher drag due to friction. After all the numbers are added up, I do not know which side wins.

As for setting an inflow turbulence value. My past experience is that it hardly makes a difference. But my cases are different in that they are fully turbulent and I have not thoroughly examined effects due to inflow turbulence.

Yes, I forgot that in k-w there is zero boundary condition for eddy viscousity.

These are contours of turbulent viscosity in the fluid. For kw steady (that converges) and kw-sst steady that oscilates

People advice me not to switch form model to model, but run transient with a fixed model. If it is a good way to fix things?

here is the close up for kw-sst for trailing edge. Also residuals for

kw-steady -> kw-unsteady -> kwsst-unsteady

Time step: (1% of airfoil chord flow travel per time step, max 10 iterations per step).

And here is eddy viscosity from S-A models, where everything is going smooth

Well, I'm glad I'm not in your shoes!

1) I'm not sure what the story is with your (i.e. Fluent's) k-omega sst transitional turbulent viscosity. The contour plot of the overall field does not look right, in my opinion. But, that is best left to a different thread. I'm not sure it effects the position you are in, unless there is something really messed up with the solution on their part.

2) I also don't understand why the turbulent viscosity values at the forward outer boundary are different for the three models. Again, I'm not sure it effects the position you are in.

You mentioned wind tunnel results, can you send me a reference to the WT results?

Last night I made some runs with a NACA 0009 at 7 degrees angle of attack to simulate your cambered results at 4 degrees angle of attack. The geometry isn't apples to apples, but it is what I had on short notice. My Reynolds number was 70000 and my Mach number was 0.1 (my solver is compressible) I used the SA turbulence model, and also ran laminar (unfortunately I did this at 4 degrees alpha).

For the SA model, I ran it without constraining the eddy viscosity, and then made some runs where I constrained the eddy viscosity to a maximum values (I assume Fluent can do the same thing if you want to try that out). Anyway, the flow becomes unsteady somewhere between a max eddy viscosity of 5 and 10. I non-dimensionalize my values by the freestream value (edit: dynamic laminar viscosity value). At see level the dynamic viscosity is 1.46e-5 kg/(m-s). Without constraint, my eddy viscosity above the trailing edge is about 24. This seems to agree with yours. I assume your problem is close to sea level temperature, thus sea level dynamic viscosity.

So, all these models are on the verge of becoming laminar in nature, at least in regards to unsteady flow, i.e. sub critical.

At your end of the Reynolds number spectrum, there are three types of flows. (what I'm about to write is more qualitative than quantitative)

For the laminar to turbulent transition region (i.e. > Re 1.0e5) I think the fully turbulent models will capture lift OK but not drag, i.e. a drag bucket. This is where the k-omega sst transitional model may actually help, assuming it works.

For sub critical flows, i.e. complete separation, running laminar may be the best way to go. In this region I expect the Cl to drop significantly from the 2pi lift curve slope.

For the region between sub critical and transition, i.e. reattached separation bubble, maybe a model would be to run a fully turbulence model and put an upper cap on the eddy viscosity. This will not give you a reattached separation bubble, but it may get you closer to the values you are looking for and maybe get the airfoil to stall as expected. The modeled viscous forces will be higher since the flow does not have a recirculation region. The pressures will be off too, but I don't dare guess in what direction. I'm not sure any of the turbulence models, L.E.S. included, will be able to reliably model this region. Of course there is hysteresis too. Expect errors. Maybe even large errors. But this is also true for wind tunnel models. The upstream turbulence for a WT can be high, thus causing the wind tunnel to behave more like natural laminar to turbulent separation. The hysteresis aspect makes it so there probably isn't a right answer.

Here are my values for NACA 0009 at 7 degrees (the moment center calculated by the code is at the leading edge NOT 1/4 chord). Also note that the Cl next to "Moments" is rolling moment, not section lift. After each set I calculate values for CD, CL, and CM at 1/4 chord. The first two data sets are for a Re of 70000 and the 3rd is for 500000 (for comparison)

Fully turbulent SA, unlimited (Re 70000):
# Pressure
# Forces: CX = -6.915001e-02 CY = 0.000000e+00 CZ = 6.946670e-01
# Moments: Cl = 0.000000e+00 Cm = -1.660774e-01 Cn = 0.000000e+00
# Viscous
# Forces: CX = 1.271649e-02 CY = 0.000000e+00 CZ = 1.425578e-03
# Moments: Cl = 0.000000e+00 Cm = -1.532532e-04 Cn = 0.000000e+00
# Total
# Forces: CX = -5.643352e-02 CY = 0.000000e+00 CZ = 6.960926e-01
# Moments: Cl = 0.000000e+00 Cm = -1.662306e-01 Cn = 0.000000e+00
CD = 2.88194e-2, CL=0.69778, CM (1/4 chord)=0.007793 (had to calculate these values by hand so there is the chance I messed up)

Full turbulent SA, limited to 10 times the sea level viscosity (Re 70000):
# Pressure
# Forces: CX = -6.617254e-02 CY = 0.000000e+00 CZ = 6.681151e-01
# Moments: Cl = 0.000000e+00 Cm = -1.552691e-01 Cn = 0.000000e+00
# Viscous
# Forces: CX = 1.240199e-02 CY = 0.000000e+00 CZ = 1.446744e-03
# Moments: Cl = 0.000000e+00 Cm = -1.970315e-04 Cn = 0.000000e+00
# Total
# Forces: CX = -5.377054e-02 CY = 0.000000e+00 CZ = 6.695619e-01
# Moments: Cl = 0.000000e+00 Cm = -1.554661e-01 Cn = 0.000000e+00
# Group[0] Total Loads
# Forces: CX = -5.377054e-02 CY = 0.000000e+00 CZ = 6.695619e-01
# Moments: Cl = 0.000000e+00 Cm = -1.554661e-01 Cn = 0.000000e+00
CD = 2.82293e-2, CL=0.671124, CM (1/4 chord)=0.01192 (had to calculate these values by hand so there is the chance I messed up)

Full turbulent SA, unlimited (Re 500000):
# Forces: CX = -6.860488e-02 CY = 0.000000e+00 CZ = 6.831320e-01
# Moments: Cl = 0.000000e+00 Cm = -1.628587e-01 Cn = 0.000000e+00
# Viscous
# Forces: CX = 3.273818e-03 CY = 0.000000e+00 CZ = 2.739189e-04
# Moments: Cl = 0.000000e+00 Cm = -3.766982e-05 Cn = 0.000000e+00
# Total
# Forces: CX = -6.533107e-02 CY = 0.000000e+00 CZ = 6.834059e-01
# Moments: Cl = 0.000000e+00 Cm = -1.628964e-01 Cn = 0.000000e+00
# Group[0] Total Loads
# Forces: CX = -6.533107e-02 CY = 0.000000e+00 CZ = 6.834059e-01
# Moments: Cl = 0.000000e+00 Cm = -1.628964e-01 Cn = 0.000000e+00
CD = 1.84421e-2, CL=0.68627, CM (1/4 chord)=0.007955 (had to calculate these values by hand so there is the chance I messed up)

As can be seen from the results above, the modeled drag increases with the decrease in Reynolds number and modeled lift seems to be insensitive to the decrease in Reynolds number. I was hoping that more of the loss of lift I was expecting would be captured. But, maybe there is less than I expect. I don't have NACA 0009 data at this low a Reynolds number. The drag could be off by a considerable amount (+/- 30%) since it is a result of a difference between uncertain CX and CZ values, i.e. CD=CX_vis+CX_press+CZ_press*sin(7 deg) where CX_vis+CX_press is negative

I don't think I can help out any further in regards to defining a good model.

What were the fully turbulent Re 70000 coefficient results you obtained from Fluent and what are the WT results at that data point?

Oh, I forgot to mention, the eddy viscosity at the trailing edge for Re 500,000 is about 160 times larger than the laminar viscosity.

Ooops, looking at my low viscous CX values for Re 500,000 I realize that I used the wrong grid, i.e. the y+=1 for Re 70,000. I was also wondering why my Re 500,000 lift result was so far from 2pi.

So here are the results for the correct grid!! Geez.

Full turbulent SA, unlimited (Re 500000):
# Pressure
# Forces: CX = -8.148592e-02 CY = 0.000000e+00 CZ = 7.283792e-01
# Moments: Cl = 0.000000e+00 Cm = -1.769565e-01 Cn = 0.000000e+00
# Viscous
# Forces: CX = 1.091467e-02 CY = 0.000000e+00 CZ = 1.058283e-03
# Moments: Cl = 0.000000e+00 Cm = -4.110901e-05 Cn = 0.000000e+00
# Total
# Forces: CX = -7.057125e-02 CY = 0.000000e+00 CZ = 7.294375e-01
# Moments: Cl = 0.000000e+00 Cm = -1.769976e-01 Cn = 0.000000e+00
CD = 1.88508e-2, CL=0.73260, CM (1/4 chord)=0.005362 (had to calculate these values by hand so there is the chance I messed up)
The eddy viscosity above the trailing edge is about 75 times the sea level dynamic laminar viscosity.

Well, that's better.

OK, a recap, RANS SA results for NACA 0009 at alpha 7.0 degrees and sea level

Re,Cl,Cd,Cm,Notes
50,000 0.67112 2.82293e-2 0.01192 (Limited to 10 times laminar viscosity)
50,000 0.69778 2.88194e-2 0.007793
500,000 0.73260 1.88508e-2 0.005362

The loss of lift and drag increase has been captured. How well, I'm not sure.

Oh, just remembered, two equation turbulence models may need less than y+=1, maybe y+=0.2. Not sure why but it has something to do with the algorithm and not physics.

Thanks a lot Martin,

For SA I got cd around 2.7E-2 and Cl around .75, but for k-w standard Cd is about 7E-2, which is completely unacceptable.

I was directed to interesting articles that consider almost exactly the same case as here (for sd7003, which is from the same family as sd7037 I am dealing with here: wind tunnel measurement data for sd7003 are in the first article below): they saying that it is extremely difficult to get decent results for drag by using turbulence models without sophisticated transitional algorithm even for conventional airfoils, not to mention other types of airfoils I wanted to analyze afterwards.

1) Computational and experimental investigations
of low-Reynolds-number flows past an aerofoil, W. Yuan and M. Khalid, THE AERONAUTICAL JOURNAL, JANUARY 2007 http://www.raes.org.uk/pdfs/3109.pdf

2) http://persson.berkeley.edu/pub/uranga09iles.pdf

Truffaldino

Cool. So it seems, when I look at your first paper, that our SA results are in the ball park of the experiment. Granted we don't have a bubble. Unfortunately, to even hope to get a bubble, the number of grid points will need to be upped drastically. And this does not lend itself to 3D. If your grid is fine enough, even a RANS solver may pick up on the bubble and reattachment. The key is that the recirculation of bubble itself creates eddy viscosity and that eddy viscosity then dampens out the flow downstream, thus causing reattachment. It is the same process which occurs in the wake of a blunt body or for airfoils at higher angles attack and higher Reynolds numbers, just on a finer scale. But you need a lot of grid points along the chord and a lot of CPU horse power.

As for the k-w standard CD value being so large, not sure what the story is with that. One thing to check is how well the k-w standard viscous CX values compare to SA values. If they do not compare well, you probably need to up the number of points in the normal direction and have a y+ value significantly less than 1, i.e. maybe 0.2.

Good Luck!

Does the latest version of Fluent not include the gamma-Re_theta (intermittency and momentum thickness Reynolds number) transition model?

I have access to fluent 6.3.26 and it has s-a, k-e, k-w, k-w sst, k-w sst transitional, and Reynolds Stress: I could not get decent results with k-w sst transitional for sd7037 at RE=70000.

I know that γ-Reθ t-transition model is purely based on local variables, will it give reliable results at Re=10^4-10^5? Is it suited for geometries other than conventional airfoils, say an airfoil with a step on a suction side?

As far as I understood from the the first reference given in the post 24 local-based predictions will not work for such reynolds numbers.

I have the same problem as yours, I want to know that your problem get solved?
the gamma R theta seems to be good enough for the problem, but it is not in fluent 6.3.26 I use.
Does anybody know that if Ansys 12 has this model or not?
http://hiliftpw.larc.nasa.gov/Worksh...-2011-0864.pdf

Truffal -

I have used the k-w (SST) γ-Reθ transition model with excellent results on the NACA 0012 airfoil at 5E4 <= Re <= 2.5E5. I have recently modeled the SD7003, as well, though I haven't checked the results.

I have seen validation studies with the model on flat plates, turbine blades, and airfoils. The airfoils were pretty complex in shape. Here are some studies:

Malan, P., Suluksna, K., and Juntasaro, K., Calibrating the γ‐Reθ Transition Model for Commercial CFD, AIAA paper 2009‐1142 (2009).
Sørensen, N.N., Airfoil Computations using the γ‐Reθ Model, Technical University of Denmark, Report Number Risø‐R‐1693 (2009). http://130.226.56.153/rispubl/reports/ris‐r‐1693.pdf
Alam, M., and Suzen, Y.B., Numerical Investigation of Transitional Flows over a NACA0012 Airfoil, SAE Paper 2008‐01‐2250, (2008).
(Be on the lookout soon for a paper from Counsil and Boulama using the SST γ-Reθ model!)

Your Yuan and Khalid paper did not discuss the SST γ-Reθ. In their paper, they used fully turbulent models coupled with the e^N method with moderate success.

Rambod -

The k-w SST transitional model is the SST γ-Reθ model.

Thanks for Info: Did you do steady or unstedy simulations, if unsteady/transient what was the timestep? What was the resolution of grid (in direction of normal and along airfoil surface) and boundary conditions for turbulence parameters. Did it model the bubble size and location of transition correctly?

I tried k-omega transitional steady and then unsteady and I have strongly oscillating residuals and messy flow in both cases. I understand that it is due to instabilityof the bubble. What is the way to get accurate results?

Will be grateful for useful info

What angles of attack did you run and did you get a bubble at the lower Re number?

Joshua,

The published papers you gave (I do not have access to one by Alam) seem to discuss flows at re of several millions (perhaps your coming paper will present results on smaller re).

Do you know other references that discuss gamma-re-theta at re=10^4-10^5? Will be grateful for informattion

Truffaldino

I have encountered several names similar to the named model, do U know (preferably by introducing reference ) which one is most suited for external flows of Rey=10e5 to 10e6 , and what y+ should be reached for answer:
Fluent in Ansys 12 :
k-Omega (2 eqn) => Standard/SST (low-Re Corrections)
transition k-kl-omega (3 eqn)
Transition SST (4 eqn)

in Fluent 6.3.26
k-Omega (2 eqn) => Standard/SST (Transitional Flow)

Truffal -

It was unsteady, but I'm afraid I can't give you the grid, timestep, parameter, etc. details because we're publishing the paper! The residuals do oscillate rather strongly, but should be oscillating at an appropriately low residual order. Monitoring another parameter of interest, like lift, is a good idea.

And yes, our paper is the only one we know of using the model at lower Re for airfoils.

Martin -

We ran from approximately 0 to 8 degrees. A bubble was seen at the nonzero angles of attack. Laminar separation without reattachment was seen at zero degrees.

Rambod -

Not familiar with Fluent. Only CFX. SST Gamma-Theta model is the one I used.

There is quite a confusion with the names of models in Ansys/Fluent.

I found another reference that has comparison different models with gamma re theta and sst-for transitional flows among them (see figure 4 there) http://stc.fs.cvut.cz/pdf/DurisMiroslav-313777.pdf

gamma-re-theta which is a 4eqn model, performs better, but unfortunately it is not in fluent 6.3. Although there is a sst transitional model in Fluent 6.3, it is basically 2eqn sst model with one coefficient algebraically depending on flow variables and is of a little use in our case.

In the link Truffal provided, they compare the classic (standard) SST model with the SST transition model (i.e., gamma-Re_theta). The SST transition model is the same thing as the gamma-Re_theta model. It has 4 equations - the 2 for the classic SST (k and w), plus the intermittency factor (gamma) and momentum thickness Reynolds number (Re_theta).

What is one looking for when choosing a good turbulence model for low Reynolds number flow?

For example, I've attached a SA (fully turbulent) run for Mach 0.10, alpha=7, and Re=5000 over a NACA0009 airfoil. My off wall spacing is 4.0E-6 (my airfoil chord is 1.0). The spacing is small and is based on having a y+=1 at 1/4 chord for a Re number of 5.0e6. The result is steady and has been converged to machine zero.

If I was looking to improve this, what would give me the most bang for the buck?

Screen shots
1) Cp and grid
2) U velocity
3) U velocity limited to negative values. Shows reversed flow, thus a bubble exists.
4) Eddy viscosity as a ratio to laminar viscosity
5) Eddy viscosity limited to 0.01. The blue areas shows the regions which are basically unaffected by eddy viscosity.

Well, truthfully, a turbulence model is not ideal for low-Reynolds-number flow. The physics is very complex, so modeling the physics is tough. Namely, RANS methods can predict neither the Tollmien-Schlichting waves nor the Kelvin-Helmholtz instabilities associated with separation-induced transition.

Certain turbulence models can predict some aspects of the flow. The SST model can predict some flows under adverse pressure gradients with possible small laminar separation bubbles, though most fully turbulent models are too dissipative to sustain the LSB. The SA model has shown some success as you have noted below.

The SST gamma-Re_theta model has built-in correlations for better transition prediction, namely equations based on the intermittency (the fraction of the likelihood of turbulence, 0 - laminar, 1 - fully turbulent) and momentum thickness Reynolds number. This model also has a built-in correlation for separation-induced transition, which is highly useful and unique. The 2 extra transport equations will cause the solution to take longer to converge. Further, the solution must be unsteady. I've had success using the models for Reynolds numbers as low as 50000, but Re = 5000 may require something more physics-based, like the e^N, LES, or DNS methods.

I am still confused: At figure 4 of that reference they list k-w sst, k-w sst trans., gamma-re-theta. So it sems that they distinguish between k-w sst trans and gamma-re-theta. At that figure k-w SST is close to k-w SST trans, which is drastically different from gamma-re-theta. It seems what they call k-w sst trans. is not SST transitional, but SST with k-omega options "Transitional Flows" from Fluent 6.3.

Martin,

Have you tried to run laminar? Is it really turbulent at RE=5000 and alpha=7? At such a low speed the transition can be delayed up to the trailing edge.