|March 26, 2011, 09:27||
Meshing a 2D airfoil properly
Join Date: Jan 2011
Posts: 73Rep Power: 7
I am doing a study of the flow around truncated 2D airfoils using o-meshes and I would like to know if you know any reference where it is explained how to distribute the cells over the airfoil (i.e--> the amount of cells in the chordwise, trailing edge and leadign edge). I have been doing 2 different meshes with different distributions and I get a difference in the lift of 5%. It is not a lot, and the results look very similar to the reference I am comparing them to. However, I want to make sure I am meshing properly.
Maybe you can give me some advices or some references (papers...) where they talk about this.
|March 27, 2011, 15:11||
Join Date: Mar 2009
Location: Fort Worth, Texas, USA
Posts: 235Rep Power: 9
Here are a couple of quick suggestions.
First, you should consider the Y+ value of the first grid point off the airfoil surface. You can find the equation for computing Y+ from a variety of sources including the internet. See if your mesh is giving you a Y+ of about 1. If you are using a wall layer model you can probably have a bigger Y+ around 30 or so. Can't remember exactly and it probably depends on the code you're using.
Also, consider doing a grid refinement study and/or Richardson extrapolation (again, you can read about this on the 'net). Basically this is just running a sequence of finer and finer meshes to see that the solution is converging as the grid gets finer.
Since you mention that you're using O-grids (structured quad grids) you might also want to ensure that you're getting sufficient resolution of the wake. That depends on the angle of attack too.
Other mesh resolution issues include chordwise resolution in the region of the shock wave if you're running at a transonic mach number.
I realize these suggestions are more general and less specific but hopefully they help.
|March 28, 2011, 03:30||
Join Date: Feb 2011
Posts: 469Rep Power: 11
In addition to what John mentioned, I would suggest playing around with the outer boundary distance. Unfortunately for 2D airfoils at subsonic and transonic speeds this can be anywhere from 100 to 150 times the chord length. One can get away with less for 3D grids, about 50 times max length dimension.
I've had resonable results using 401 points around airfoil and 801 points in outward direction with a y+=1 at the quarter chord location for a NACA 0012. I also clustered the points around the leading and trailing edge, about 4% of average point distance for leading edge and 2% of average point distance for tailing edge. But my trailing edge was sharp. For transonic results, this may not get you a crisp shock. This may not affect the overall integrated results much but will affect how your pressure distribution looks.
On the other hand, if you are trying to capture a separation bubble, you'll probably need to use more points. I am also assuming you are running Euler or turbulent and the results are steady. Unsteady results may need for points.
|Thread||Thread Starter||Forum||Replies||Last Post|
|Airfoil Meshing Scheme in Gambit||J. Weiler||FLUENT||6||October 2, 2011 15:41|
|[Other] Ansys meshing airfoil and / or compressor blades||baw192||ANSYS Meshing & Geometry||8||September 23, 2011 00:43|
|Oscillating Airfoil - Dynamic meshing or user-defined velocity profile.||DarrenC||Main CFD Forum||5||July 19, 2010 22:33|
|[GAMBIT] Meshing airfoil using .dat file problem||creggie||ANSYS Meshing & Geometry||10||June 27, 2010 19:24|
|Help regarding basic airfoil meshing in CFX||amoolraina||ANSYS Meshing & Geometry||2||May 22, 2010 18:51|