[alex_k1997]

I am new to ANSYS CFX and I am trying to simulate the wingtip vortex downstream a NACA0015 wing. However, the magnitude of the vorticity downstream the wing is significantly lower than the experimental data I am trying to validate against (I compare normalised vorticity ωc/U). I am using steady state and I have tried different turbulence models without any big difference in the results. How can I ensure that the magnitude of the vorticity is maintained downstream the wing?

[ghorrocks]

Have you done a validation and verification? There is a lot to check (see FAQ https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F), but the big ones are to ensure your mesh is fine enough and convergence criteria tight enough.

Also make sure you consider numerical issues: dissipative advection scheme like upwinding will cause this sort of problem. I would set it to second order advection (Use Hybrid differencing with a blend factor of 1.0), or maybe use QUICK or other more sophisticated schemes.

Also look at your turbulence models. Many 2-eqn turbulence models over damp these sort of vorticies. Look at the curvature correction model for SST, and also consider RSM models.

[alex_k1997]

I have read some things about vorticity confinement. Is there a chance that I need to use something like this and if yes how can I implement this in CFX?

[aero_head]

Hello,

As ghorrocks mentions, you need to consider damping for these types of problems.

Other than that, looks like vorticity confinement would work. I found a paper goes over a scenario like yours: https://www.researchgate.net/publica...rotating_blade. In FLUENT, you can implement a UDF (user defined function) and specify a confinement parameter.

Here is another paper that covers more of the theory of confinement: https://www.researchgate.net/publica...ty_Confinement

[ghorrocks]

I just looked up Vorticity Confinement on Wikipedia - it appears to be a special CFD approach designed for modelling flows with lots of vorticity. This approach may be useful in your case - but you won't be doing it in CFX. This sounds like something you will need to write your own CFD code for.

But CFX is quite capable of accurately predicting your flow. You just need to do the validation and verification stuff I described in my previous post.

[alex_k1997]

I have done a mesh independence study and my mesh gives the same results with meshes of 12million cells up to 50million. Here I attach a screen shot of my Vorticity monitor points. Point 1 is at the wingtip x/c = 0 and monitor point 2 at exactly 1 chord downstream (Screenshot 1).

I have tried RSM with no difference in the results. However, I still don't understand how to use curvature correction. What production correction value do I need to use? (Screenshot 2)

Also, I use an inlet normal velocity of 7.85m/s with air at 15degrees and my wing chord is 0.2m. Therefore my Reynolds number is about 10^5. However, in the solver is says that my Global length is 2 and indicates a Reynolds number of 10^6 (Screenshot 3). Why is this happening and does this Reynolds number affects my results?

Screenshot 2021-02-20 at 6.58.53 PM.jpg

Screenshot 2021-03-08 at 9.43.19 AM.jpg

Screenshot 2021-03-08 at 9.48.23 AM.png

[ghorrocks]

I cannot see your mesh sensitivity results. A factor of 4 difference is a bit small, a factor of 8 to 10 is more normal. Also have a look at the grid convergence index mentioned in the FAQ.

You have not tried second order differencing as I recommended in my first post.

Strange that RSM was similar.

Read the documentation on curvature correction. Just leave it at defaults unless you have a good reason to do otherwise.

The solver calculates the global length as the cube root of the volume and uses that to calculate the Reynolds Number. It does not represent the airfoil Reynolds Number like you have calculated, it is global averaged Reynolds number to just give a general idea about what regime the simulation is in. Do not confuse this global Reynolds Number with a specific application Reynolds Number, like your airfoil.