Has anyone had accurate success in modelling 2-D airfoils/wings in Fluent? If you have, what turbulence model did you use and what type of grid/boundary layers did you use? My results have not been very encouraging using various setups, and I would appreciate any hints anyone might have.

Thanks in advance.

D.Brown

Hi there, I used Fluent to simulate the flow past a NACA0012 airfoil and compared the results with experimental data. The agreement was satisfying. The point is, that even for this airfoil, being used again and again as a test-case, it is difficult to find appropriate data. You can find data for pressure distribution easily but skin friction data etc. is more difficult, although available.

My experience is: RNG-k-e Modell Two-layer at the wall Turbulence Intensity and Characteristic length is important. Distance of outer boundary from airfoil is important.

Simulations done using a hybrid mesh, ie. quad-cells in the boundary layer region, triangular cells in all other regions. The boundary cell layer should be thick enough and you must take care of your y+ along the profile.

Good luck Detlef

Please contact your support engineer. We have some validations for airfoil flows.

As far as airfoil flow predictions are concerned, things can go wrong you when;

- You underresolve the leading edge, i.e., the curvature near the leading edge - The domain is not large enough and you impose far-field boundary conditions on the "no-so-far" boundaries - The boundary layer (and near-wake) is under-resolved. Especially when the mesh is too much stretched in the direction normal to the wall - A laminar-turbulent transition occurs over a significant portion of the airfoil and you want to match drag coefficient at very low angle of attack - Incidence angle is such that stall occurs

Please check your setup with this list in mind.

Good luck

(1). This is a very good question, because it represents a practical external flow problem. The opposite is the internal flow problem, which has even more complications. (2). In the airfoil case, there are three basic parameters, namely, a). the Mach number, b). the Reynolds number, and c). the angle of attack of the airfoil (AOA). (3). In the incompressible flow limit (Mach number=0), and for the low Reynolds number (say, Re=<100), with small angle of attack, one will get very smooth flow over the airfoil. In this case, one should extend the outer boundary as far as possible to simulate the real free-stream condition. The mesh density near the wall should be moderate. And one should always check out this case first. Mainly to give him some confidence. (the evolution of the political system also follows the same principle) (4). The next step is to increase the Reynolds number and also increase the mesh density near the wall to obtain another solution. As the Reynolds number is increased, there is no need to change the outer boundary condition position. Because the viscous displacement effect will be reduced when the Reynolds number is increased. You may have to add more mesh points in order to achieve the mesh independent solution. (5). The Reynolds number can then be increased to several thousands, or even up to 1E10+4, 1E10+5, etc, as long as the converged solution is achievable. Naturally, you will run into the transient flow problem or the convergence problem if the steady state equation is used. (6). At ,say one thousand Re, the flow around the leading edge will turn into turbulent flow following a transition region. To be realistic, one needs to switch to turbulent flow calculations. (7). So, the basic need there is to have a turbulence model which will handle both the laminar flow region and the turbulent flow region. This is an advanced task. (8). So, normally, one will assume that the flow over the boundary layer is fully turbulent. This may be realistic, if the Reynolds number is high and the laminar flow region near the stagnation point is very small. Or the boundary layer is tripped into the turbulent flow. (9). With the experience learned from the high Reynolds number laminar flow calculations, at this point, he should have some feeling about the mesh density distribution next to the wall. One has to develop his hands-on experience in terms of the mesh density distribution. Then, he should be able to pass the turbulent flow simulation easily. (it took thousand of years for the Greeks to develop the political system) (10). Since the turbulent boundary layer will cover a much wider region than that of a laminar flow, more mesh points are needed here. Normally, if one has 60 points across the turbulent boundary layer, he should be able to get good resolution, thus good results too. This does not cover the external flow field mesh points. So, if one has over one hundred points from the wall to the outer free stream, he should be able to get good answers. (11). At this point, one has achieved only a small step in computing the real flow over an airfoil. (12). If one increases the angle of attack, the flow field will get worse, and it will become more difficult for the turbulence model to handle it correctly. (13). If the flow separation occurs, then one is really heading for trouble. (14). As the Mach number increases to transonic, a thin shock will form, and it will create shock wave/ boundary layer interaction problem. These high gradient regions require adaptive meshing to correctly capture the flow features. Then, the turbulence model used also need to have the capability to handle this compressibility effect. It is not easy at this point. (15). In the internal flow of a gas turbine blade calculations, the heat transfer is very sensitive to the flow transition, and the problem will become really messy. (16). These are evolutionary steps one has to go through in calculating the flow over an airfoil. (at one time, two years ago, it took me two weeks to adjust the mesh so that a trailing edge shock in the transonic flow could be properly captured. With coarse mesh, you can't see it) (17). That's a long story for a seemingly simple external flow over an airfoil. Good luck and Have a nice trip.

Dear Mr.John C. Chien,

How are you, I am using FLUENT5 to simulate the unsteady flow of 2D airfoil & 3DWing,but I meet a problem when I model 2D airfoil mesh, I don't know how to control the mesh density near the wall by using structure mesh(quad Map method). Is it possible for Gambit to model structure mesh? and How? I don't know why I could not transfer boundary layer generated by Gambit to Fluent 5? Is there technique?

Thank you in advance!

(1). see Gambit training notes, modeling a mixing elbow(2-D), mesh-edge-mesh edges-grading. (2). Right now, I am not using the code, please ask Fluent support engineer for sample tutorials and help. good luck.