3D NACA0012 airfoil with Endplates

Hi everyone,

I have been working on a simple project - https://www.simscale.com/workbench/?pid=3556489279416324644&mi=run%3A32%2Csimulation%3A14&mt=SIMULATION_RUN - running a 3D NACA0012 airfoil with endplates. I have previously done this without endplates and obtained values much less than the 2D experimental values which I expected due to the low aspect ratio used and hence the vortices at the wing tips are having a much larger effect on the spanwise pressure gradients. I also did this with an aspect ratio of 5 and there was much stronger agreement with the quasi 2D results. The results I am trying to compare with are shown below.

I have ran this simulation with endplates and was expecting to see a larger coefficent of lift, something closer to the values in the image attached for varying angle of attack.

I’m not really sure where I have gone wrong. Is it that my geometry is not watertight or my boundary conditions arent as they should be?

Any advice or comments are all welcome as I am struggling to see what I have done wrong.

Thank you,

CFD Squad, can you see what Pippa can do better?

Thanks a ton!


Hi @pippatreacy123,

There are many problems with your simulation:

  1. Mesh did not create any BL. Fixing it will take time. Look at examples in @dschroeder and @DaleKramer projects.
  2. Wake zone should also include the wing TE and plate TE.
  3. Side walls should be set as slip BC, not as outlet. You can also use Custom BC, setting all input fields to Zero gradient (you have huge simulation domain, so flow which is at AoA 4.2 degrees will not reflect on those side walls).
  4. When you see in your log files that k and omega have 0 iteration, you simulation is not solving those essential parameters. look also at Convergence Plot: k and omega are flat after about 200 steps. You can mend it in ‘Numerics > Residual controls > Absolute tolerance (set to lower values)’.




Hi Retsam,

Thank you for these tips, I have been working on the mesh today.

If I change the tolerances for k and omega to have lower tolerances but find that I am getting no iterations for omega, what would this indicate?

Many thanks!

It can mean you need less steps in your simulation to converge to stable results. You can still lower the tolerance separately for omega, but forces will be not impacted, but wake shape may change a bit.



Okay perfect, thank you.

Additionally, I have fined the mesh in a different copy - https://www.simscale.com/workbench/?pid=3356757880119779606&mi=spec%3A07970ea4-e5dc-41f0-a1cf-f62e95f2d2c4%2Cservice%3AMESHING%2Cstrategy%3A28&sh=14

I used a first cell thickness of 0.0000222839741079746 with an expansion ratio of 1.5 and 7 layers. The mesh I have is as below.

I am still off on my coefficient of lift and drag values. Is it that my mesh is just too coarse following the boundary layers?

No, your mesh is not too coarse. End plate is a blunt body, did you account for it? Do you calculate CD, CL separately for airfoil and end plate?

Obtaining CD / CL matching experimental results is very difficult and for AoA > 12 degrees near impossible.

You can looks at one of my study of NACA0012 using TET mesh for AoA 11.15 degrees, with different domain size. That study aims at quasi 2D setup, but has no description of preliminary studies I did (for NACA0012 AoA 4 - 10 deg).

Essential learning is that the mesh should be refined for high gradient pressures on airfoil surface…

Take care,


Hi Retsam,

When you say account for the end plate being a blunt body, what are you referring to in terms of my set up or meshing method? I did not calculate these separately, should I, and if so why?

I will have a look at your study now to see if I can get some inspiration for my mesh :slight_smile:


Simply CD induced by your ‘end plate’ will be big and will bias the CD of the airfoil with end plate. You can select different faces of your geometry and calculate separately acting forces…

Take care,


Hi Retsam,

Thank you for all the help so far.

I am still curious to understand why my results are so far off the 2D experimental results due in the fact that I have an endplate on the airfoil. My coefficient of lift is 0.169 and I was expecting around 0.452. I would have assumed that having the endplate this would have reduced lift-induced drag effects and improved the lift curve slope.
For Run 8 in the link below, my k and omega value are still not iterating but I think I am happy with the mesh I have achieved. Any further advice would be greatly appreciated.

Many thanks,


I’m slightly confused about the layer settings that you have. You don’t have result controls for y+ but, from my calculations, you should have y+ = 1~ right now. That would require a full resolution wall treatment instead of wall functions.


Also the transition from layers to surface cells is not very smooth. You’re getting a huge jump in terms of cell size:

Some courses of action would be:

  • 1: try to re-run using full resolution;
  • 2: create a wall function mesh (a first layer thickness of around 0.00065 should give you y+ = 40-50~). This way you can also try to get a smoother transition.
1 Like


Thank you for the suggestions.

I have tried them and still no success.

Additionally k and omega seem to still converge within 50 iterations and then flatten out. Why is this?