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?