2D External flow over NACA0012
 

Hello,

I have searched quite a bit on this topic and there is admittedly a lot of information out there. But I do have a question regarding some of my preliminary results which are coming in.

I am doing a 0-90 degree AoA sweep in external domain using CFX with a 1 element thick 2D model and periodic walls. First layer thickness is still being investigated (shooting for Y+ of 1), my colleague initially started using an unstructured mesh but we may switch to a structured ICEM mesh soon.

The Cd and Cl coefficients I am getting show stall taking place at a much later AoA than data shows.

I believe that the drag coefficient for a flat plate is approaches about ~2 when aspect ratio of a plate approaches infinity (2D case). Therefore, since the NACA0012 acts like a flat plate when 90 degrees into flow, should I not be getting a Cd of about 2? I am seeing in fact a higher Cd and a much later stall angle than shown in data in these simulations.

Couple things I want to do to help increase fidelity:

1. Tighten up my first layer thickness
2. Turn on transitional turbulence (although i dont think this will matter for angles past stall??, please let me know if im wrong on this).
3. switch to structured mesh

I think that CFX is having a hard time dealing with modeling the separation at low AoAs, if anyone has any other ideas please let me know.

Thank you,


:cool:

The 90 values will be dependent on Re to an extent, but, yes, the ball park number for Cd at 90 degrees for a normal non fat airfoil is 2.

http://hdl.handle.net/2060/19930084501

I gather your question is about 90 degrees, even though you mentioned separation at low AoAs.

In general, you should not have problem determining separation of an airfoil at 90 degrees. It will separate at the leading and trailing edge. Your drag should also be relatively independent of y+, at 90 degrees. Within reason. The bigger issue is capturing the wake on the lee side. I also assume, for your 2D shape, that the flow is unsteady on the lee side? Both structured and unstructured solvers should give you similar results at 90 degrees AoA. Also, the turbulence model could give you noticeably different results. The reason is the amount of eddy viscosity that is created. The more eddy viscosity, the more stable the results will be. If there is enough eddy viscosity, you may get a stable result when the result should be unstable.

Thank you for the insight.

So when is a good time to use transitional flow if I am not sure what the steadiness of the solution should be?

Also, I am doing a full 0-90 sweep on AoAs. So I really want to try and capture that separation of this airfoil to at least 15% accuracy for Cl @ stall.

I dont want to turn this into a science project, meaning; too much fidelity will take too long and this project just needs ballpark figures for airfoil performance.

For now, the model is predicting stall at like 30 degrees when in reality it is well documented to happen at about 12 degrees for this airfoil at high Re's.

What else can I do to try and close the gap on stall point validation and basic overall increases of fidelity for a 0-90 aoa sweep for this airfoil at high Re's??

Thank you,

:cool:


I forgot to add this is modeled as unsteady with timesteps of 0.2s and Re in the 10^7 range. I will be calculating the required timestep to allow good solution convergence and to keep flow from blowing through 20 elements at a time if the timesteps are too big etc..

OK, I'm confused. Your airfoil stalls at 30 degrees? I'm assuming your flow is incompressible/low subsonic and not high supersonic/hypersonic.

If your airfoil stalls at 30 that would put lift, for something like the 0012 at incompressible high Re, in the ballpark of 2.8. What is your Cl value?

I have Mach 0.3, Re=3.0e6 results that stalls in the ballpark of 14 degrees with a Cl of 1.34 using Spalart Allmaras. The results are steady and converge to machine zero. This is using my code, Aero Troll.

Sorry, I don't have an easy answer or even a rule of thumb. In general one must find shapes that are similar to the one being analyzed and use those to bound the problem or gain insight into it. It takes a lot of work to nail down uncertainties.

Flow is moving very slow, fluid is water so incompressible. Re is very high due to size of the airfoil.

I will take a look tomorrow at what our predicted Cl and Cd is at 30 degrees. Cd is closer to data match but Cl definately does not match the data.

Do you think that because this airfoil is 2D that it has something to do with the skewed results? Just like flow over a flat plate with infinite aspect ratio shows a Cd of 2 vs flow over a flat plate with aspect ratio of say 10, about half that approximately ~1? What do you think of that?

Thank you

Sorry, at the moment I think there is something I am unaware of. If your airfoil is 2D, which it sounds like it is, then it should stall somewhere around 12-15 degrees.

BTW, why do you model your side walls as periodic? I know very very little about CFX, but usually the sides for a 2D case are set to symmetric or some specific code unique B.C. which implies a 2D case. A periodic B.C. might allow for cross flow to exist. If this was the case, then the airfoil might not stall till later.

Yes my mistake the side walls were set to symmetric not periodic.

What else do you think I should do?


EDIT: Should I reduce the timestep size to get a courant number near 1? Will this help the solution accuracy?

Not sure what might be going on, so here are things I try to do.

1) I would guess that CFX has an example of an airfoil. Play around with that by changing, one at a time, input values to reflect your case.
2) In general, for a 2D case, I like my outer boundary around 150 times my chord. But 50 should be reasonable. I would definitely not get closer than 20 times, unless I'm just doing preliminary runs.
3) Assuming a wall function is not being used, a y+ of 1 at about 10 to 20 percent of the chord length. My first off wall spacing would be constant along the airfoil. I do not use wall functions. I will also do a few runs with y+ of 0.5 to insure that my solution doesn't change much.
4) Usually I use a structured grid solver so my grid would be a C grid. An unstructured grid does not need to be C. You need to get enough cells next to the body, especially leading and trailing edge. You'll also want to capture the wake near the airfoil.
5) The code I use is a compressible solver, so my farfield B.C. would be Riemann. For an incompressible solver a boundary condition which sets velocity and extrapolates pressure on inflow and sets pressure and extrapolates velocity out outflow is usually used. Your documents should give an example. However, if your boundary is far enough away, setting the outer boundary to freestream values should work, though with a little error.
6) I usually use Spalart Allmaras. That should be OK at Re 1.0e7. You may be off with friction drag a little, but it should still stall at about the right point. For your case, at stall, a solution with SA would probably be steady.
7) In general, for steady state runs, I converge a few runs to machine zero to nail them down. Sometimes significant changes occur, even at low residual levels. However, that normally is not the case with a 2D airfoil. But never hurts to be certain.

In regards to your questions about converging the problem, if you are able to converge the problem to machine zero (i.e. it is steady state), then changing the rate of convergence probably will not change the solution.