# Modeling Backflow for a 3D Airfoil (Wing of Finite Span)

 Register Blogs Members List Search Today's Posts Mark Forums Read

 August 11, 2009, 14:54 #2 Senior Member   Joshua Counsil Join Date: Jul 2009 Location: Halifax, Nova Scotia, Canada Posts: 366 Rep Power: 17 I just tried running the simulation with a 5 degree angle of attack (rather than 15) in order to avoid stall effects. Here's the result: http://picasaweb.google.com/lh/photo...eat=directlink Clearly, there is no backflow present (or it is so minute that it is negligible). Any help? Please and thanks.

 August 11, 2009, 16:47 #3 Senior Member   Joshua Counsil Join Date: Jul 2009 Location: Halifax, Nova Scotia, Canada Posts: 366 Rep Power: 17 The solution hasn't been converging, I just realized. I did a quick Solver analysis to guess the issues. The v-Mom and w-Mom residuals did not converge. Here are the locations of the maximum residuals: +--------------------------------------------------------------------+ | Locations of Maximum Residuals | +--------------------------------------------------------------------+ | Equation | Node # | X | Y | Z | +--------------------------------------------------------------------+ | U-Mom | 229483 |-9.187E-05 | 8.038E-06 | 5.001E-01 | | V-Mom | 235721 | 1.195E-03 |-7.901E-03 | 5.001E-01 | | W-Mom | 83248 | 2.454E-02 |-2.934E-02 | 5.000E-01 | | P-Mass | 214056 | 3.267E-02 |-2.520E-02 | 5.001E-01 | | K-TurbKE | 152221 | 6.814E-03 |-1.622E-02 | 2.301E-01 | | O-TurbFreq | 22473 | 4.634E-02 |-3.962E-02 | 5.000E-01 | +--------------------------------------------------------------------+ As seen above, most of the maximum residuals are at approximately [0, 0, 0.5], which is the location of the vertex of the airfoil's leading edge: http://picasaweb.google.com/lh/photo...eat=directlink Also, the maximum residuals are significantly larger (at least 1E2 x larger) than the RMS residuals, further leading me to believe that the problem is in a local region (i.e. the vertex of the leading edge). With my current turbulence models (SST or Omega Reynolds Stress), could there be something wrong with my meshing, or am I way off here?

 August 11, 2009, 19:12 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143 Here is some initial comments: http://www.cfd-online.com/Wiki/Ansys...gence_criteria To get an accurate simulation you need to ensure your simulation is mesh, timestep and residual converged. If you have not checked the accuracy of these three parameters (or mesh and residual in steady state) then you are just getting random numbers. Glenn Horrocks

 August 12, 2009, 16:02 #5 Senior Member   Joshua Counsil Join Date: Jul 2009 Location: Halifax, Nova Scotia, Canada Posts: 366 Rep Power: 17 In the link you provided, I have completed most of the steps: I have read the Help file section on obtaining convergence and have diagnosed my problem based on its suggestions. I used monitor points to monitor the u-velocity along the span-wise side of the airfoil at different points to see if it was ever negative (indicating backflow), but to no avail. I used a larger physical timescale by using the residence time as my physical timescale. (I found the residence time by creating a streamline in Post, and used the maximum value from "Time on Streamline 1" in the "Variables" tab as the residence time.) Convergence was still not obtained. I coarsened my mesh around the airfoil. This allowed convergence to occur, but with less accurate results (and still no backflow is present). When I suppressed the inflation effects, the solution converged. When I left inflation unsuppressed and suppressed the line control, the solution did not converge. This leads me to believe that inflation could be causing the convergence problems. The physics are correct - it is a simple simulation - flow through a rectangular domain over a 3D airfoil. Backflow should be seen on the sides. I used a seemingly appropriate turbulence model, so I cannot see what is wrong in that respect. About the only thing the aforementioned article recommends that I haven't done is run the simulation as transient, but I can't see this as being necessary. Any further suggestions, comments, or ideas?

 August 12, 2009, 23:06 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143 Hi, Small backflow regions like this tend to be transient. You may be forced to run transient to resolve them correctly. When you coarsen the mesh you are simply not able to resolve them and it converges much easier. These small backflows also tend to be very sensitive to freestream turbulence levels, surface roughness, geometric abberations and other details which are difficult to control. Glenn Horrocks

 August 13, 2009, 10:28 #7 Senior Member   Joshua Counsil Join Date: Jul 2009 Location: Halifax, Nova Scotia, Canada Posts: 366 Rep Power: 17 Thanks for the help, Glenn. I owe you a virtual beer. I'll try running the simulation as transient and see how it goes. Josh

 August 13, 2009, 15:04 #8 Senior Member   Joshua Counsil Join Date: Jul 2009 Location: Halifax, Nova Scotia, Canada Posts: 366 Rep Power: 17 I ran the simulation as transient with adaptive time steps. There are no backflow or trailing vortex regions. Any clues?

 August 13, 2009, 18:24 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143 The vorticies may take some time to develop. Try using a run which has the vorticies as an initial condition and see if the transient run keeps them going or if they disappear. Also, I assume you have done all the normal checks on mesh sensitivity, adequate convergence and now you are considering transient simulations timestep size. These all need to be OK for the simulation to be accurate.

 August 18, 2009, 11:31 #10 Senior Member   Joshua Counsil Join Date: Jul 2009 Location: Halifax, Nova Scotia, Canada Posts: 366 Rep Power: 17 I have produced trailing vortexes along the side of the 3D airfoil. Success! Backflow, however, still remains very small (roughly only 1 mm from the wall) or non-existent, depending on the simulation method. After trying several different methods (parameterization, various methods of convergence, turbulence modeling, mesh refinement, transient runs, physics checks, etc.) of obtaining significant backflow, none seem to prevail, despite that the various solutions have converged. I am beginning to suspect that perhaps very little backflow along the side is to be expected. Thanks for all the help! Any further comments or suggestions are welcome.

 Tags 3d airfoil, backflow, separation, turbulence, wing