separated boundary layer ( Driver ): something wrong with komegaSST ???
1 Attachment(s)
Hello,
I have a problem concerning the Komega SST turbulence model in openfoam. I tried to simulate the separated boundary layer flow with adverse pressure gradient by Driver from: Driver, D. M., "Reynolds Shear Stress Measurements in a Separated Boundary Layer Flow," AIAA Paper 911787, from the AIAA 22nd Fluid Dynamics, Plasma Dynamics, and Lasers Conference, June 1991, Honolulu, HI. This testcase also appers in most of Menters papers about the SST model (AIAA Paper 932906; AIAA Journal 32/8, pp.15981605). Meshes for the testcase and reference data from a NASA simulation with CFL3D are provided here: http://turbmodels.larc.nasa.gov/driver_val.html You can download my setups for this case at ftp://ftp.lrz.de/transfer/of_testcas...unction.tar.gz ftp://ftp.lrz.de/transfer/of_testcas...unction.tar.gz I used the medium grid from the NASA page for my simulations. http://www.bilderload.com/daten/export8X0ZW.jpg As you can see from the attached picture, the development of cp is predicted wrong. The separation is not simulated properly with openfoam. I ran the same simulation in Ansys CFX, Fluent and Tau (DLR) on the medium grid, and these codes gave exactly the same cp curve as the NASA simulation data from CFL3D for the finest mesh. So I think there is something wrong with the komegaSST model. The cp curve is similar to the komega curves published at the NASA description page. So I think there must be something wrong with the shear stress limitation. Has anyone a clue? Some additional information to my attached openfoam setup: For the material properties i choose properties similar to that of water (dens 1000kg/m^3, kin. viscosity 1e6 ) the inflow and initial values of the turbulence variables are set according to the guidlines of Menter, which are: omega between U_in/L and 10*U_in/L k between 1e5 U^2/Re and 1e1U^2/Re with L=1 meter, Re=2000000. In the simulations I choose the lowest of the suggested values for k and the highest of the suggested values for omega, because in the simulations the boundary layer at x= 0.3m was thicker than told in the NASA description, and i hoped to retard the development of the boundary layer and to come close to the suggested results with my choice of inflow values. I also tried different values, but the inflow values appeared to have not much influence, anyway. At the wall i used omegawallfunction for omega in all openfoam simulations. For the other turbulence variables I tried a setup with kqRWallFunction for k and the Spalding wall function for nut (see picture), and a setup with fixed value conditions close to 0 for k and nut. The resulting cp curves where almost identical. For the postprocessing i used Tecplot 360 2013. The discrepancies of the SST model to the other codes seem like a real problem to me. So please help me. 
What are your yPlusvalues?

1 Attachment(s)
For the wall function setup, openfoam gave:
min: 0.00411009; max: 0.467774; average: 0.184946 For the other openfoam setup without wall function i couldn't find a way to get the yPlus values. On the same grid, Ansys CFX gave a maximum yPlus of around 1.33 . I think the most important thing to remember is that all the curves in the picture are the results of simulations with the same grid (exept the NASA CFL3D calculation, which took a finer mesh). In CFX, even on the most coarse grid the cp curve showed no big difference (see picture). 
Hello koderer,
I had just a quick look at your setups and two things came to my mind: a.) you're using upwind/linearUpwind for the divergence schemes. Upwind is only first order, so maybe your discretization error is still too big for your finest grid which might explain the differences? The other codes probably use higher order schemes. Did you perform a grid independency study to rule out discretization errors? b.) in fvSolution lower the tolerance for the omega equation to something like 1e20. Omega usually "converges" pretty quickly and the equation isn't solved anymore then which leads to inaccuracies. Greetings Felix 
Hi Felix,
Thanks for your hints. I tried the omega tolerance of 1e20 and checked that turbulence equations are solved. Didn't make much difference for cp. In the CFX and Fluent calculations i also used first order numerics for the turbulence (the other equations high resolution). And according to the CFL3D guide CFL3D also uses first order upwind for the tubulence variables. So i don't think that's the difference. If i have time i'll try the other meshes from the NASA page to check for mesh dependence. Greetings koderer 
Hello koderer,
yes, mesh dependence seems important to me, because the linearUpwindscheme didn't show second order behaviour in my tests. Maybe try limitedLinear instead? Another (possibly trivial) question: did you check for convergence using an integral quantity or cpprobe? Maybe the solution has not yet converged properly, although the residuals are quite small. Greetings Felix 
2 Attachment(s)
Hello koderer,
there has to be something wrong with your setup. I simulated the case on the second coarsest (!) grid and I get a very good agreement between OpenFOAM and CFL3D. You find the plot and the case (without mesh) attached. Greetings Felix 
1 Attachment(s)
Hello Felix,
Thanks for your case setup. I tried it and looked for the differences to my setup. I found that i accidentally didn't use the fixed value inlet boundary condition with a value of 2e11 m^2/s^2 for k but a turbulence intensity condition with a value of 0.05 (which corresponds to k=0.015 m^2/s^2). After i corrected that and took fixed value 2e11 for k inlet i received a cp curve close to that of CFL3D (see picture). For the curve in the picture, i took the medium grid and simulated 5000 iterations (It's the wall function setup i posted, but with the inlet condition for k corrected). So everything seems to be ok now. I'm glad that now i know what was wrong with my setup. Thank you, Felix. You really helped me. Greetings, koderer 
All times are GMT 4. The time now is 02:47. 