Hellow everybody! I have calculated the transonic aerodynamics of supercritical airfoils(RAE2882, DLBA186 etc.) and DTE airfoils(DLBA243, DSMA523 etc.) by using FLUENT5. The Spalart-Allmaras turbulence model has been used for every case. But, my study has some problems. First, when comparing with experimental data,the coefficient of drag is so higher than experimental value. Second, for same the coefficient of lift, the location of shock was repeatly delayed to downstream, because of lower angle of attack. And "y+ = 10" Is it proper or not? All are welcome! thank you.

(1). For the y+=10 value, you need to check the user's guide to see whether it is consistent with the model and the numerical method of the code. (2). As for the comparison with test data, I think, it is not very important. (3). It is more important to go through the "mesh independent solution" exercise first to make sure that you have the converged and mesh independent solutions. (4). After that, you can write a report or a paper to document the results and the comparison. By the way, your results should be different from the test data. If you can get good pressure distributions, you are in good shape.(at least in the area ahead of the shock )

Dear client,

In general, it is much tougher to accurately predict drag than lift, especially at low to moderate angles of attack, because drag is usually a very small quantity. And predicted drag can be sensitive to the mesh being used. So, I agree with John that some of your time needs to be spent to rule out mesh-dependency of the solution before you draw any conclusions. Here're some tips I hope will help you with your investigation.

- Does your mesh resolve the leading-edge curvature accurately enough ? You should have sufficient number of mesh points around the leading-edge. - Is your mesh fine enough to resolve, if any, the shock? More often than not, I find meshes people typically use for airfoils unduly coarse in the neighborhood of shock position (the mid-chord in the case of RAE2822 ?), probably because they cluster mesh points near the leading-edge and attempts to keep the mesh size within certain limit by using too aggressive stretching in the chordwise direction. - Does your mesh resolve the boundary layer ? Especially, you should avoid using too aggressive stretching (say >1.5)in the normal direction. - If you're using 100% triangular mesh, you may want to consider using hybrid mesh (quad mesh near the airfoil and tri. mesh in the far field) or all-quad mesh, which will provide same accuracy with less number of cells (because you can use reasonable high aspect ratio quad mesh). - y+ = 10 doesn't seem to be ideal, for y+ = 10 is in the buffer region for most of equilibrium turbulent boundary layers. I suggest you make y+ at wall adjacent cells either smaller (y+ = 1) if you're going to use low-Re models (Spalart-Allmaras model), or larger (y+ > 30) when you are going to employ wall function approach.

Even after you took great care in all this and ensured that your solution is mesh-independent, drag predictions for some airfoils could still be disappointing possibly for one of the following reasons

- When you are modeling an airfoil different from what was actually used in the experiment. stock airfoils may get distorted over time. - When the boundary layer is not tripped and the model airfoil is flash smooth. The flow in the experiement may in fact undergo laminar-turbulent transition on a substantial portion of the airfoil. - When the boundary conditions you're using do not adequately represent the experimental situation. Wall effects (blockage, effective angle of attack, etc.) can play a significant role. - When the flow is such that the turbulence model you're using falls short of representing the turbulent boundary layer in question. Try other turbulence models as well, for instance, realizable k-epsilon or Reynolds-stress model.

I hope this will help.

(1). One of the best feature of the code for the unstructured mesh is its adaptive mesh refinement options. (2). As I recall, a few years ago, it took me a couple of weeks of continuing mesh refinement to bring out a transonic trailing edge shock (M~1.2 locally) for the computation of 2-D flow over a HP turbine blade. (3). So, don't hesitate to use the mesh refinement in any transonic flow calculation. A slight error in the solution will change the shock formation condition and its location.

Hello. I am sorry that I'm not able to help you with your problem, but I was hoping someone could help me with mime.

I have a very round car (1970 Volkswagen Beetle) and I want to know what I can do to keep it close to the ground without lowering it too much. I was told that if something has a very round top that in order for it to lose drag is to have a flat bottom. Is this true? I didn't know for sure so I started to study other cars that are more streamline, then small airplanes. I see where this can be true, but I'm wondering how I can apply this information to my project. If you have any answers for me that would help, I would be fully appreciated. If there is anything that I could do to help you with your problem, please let me know.

Thank you and good luck. Sorry that I don't have a E-mail address yet for you to contact me; I'm working on that currently.