Please see the following paper: 

https://www.researchgate.net/publication/311276386_THE_EFFECTS_OF_CYLINDER_AT_THE_LEADING_EDGE_OF_AIRFOIL_NACA_0012_ON_THE_BOUNDARY_LAYER_SEPARATION?_iepl%5BviewId%5D=OzDEywmAYRaJQ3TrFqqHjoZ9&_iepl%5BprofilePublicationItemVariant%5D=default&_iepl%5Bcontexts%5D%5B0%5D=prfpi&_iepl%5BtargetEntityId%5D=PB%3A311276386&_iepl%5BinteractionType%5D=publicationTitle

Good luck

Article THE EFFECTS OF CYLINDER AT THE LEADING EDGE OF AIRFOIL NACA ...

Your equations for cl and cd are correct; I think the prior poster read them incorreclty.  In 2D, the "Area" must become a "Length", hence the chord rather than the area.  The differences in the coefficients between the NACA0015 and NACA0012 come in because the dimensional forces themselves are different - you don't get the same lift or drag for both at the same angle of attack.  There should be a guide in Fluent for running 2D airfoils; I do not run that code myself, but your assumptions look fine to me.

As for your results, it is likely that a) you are running the incorrect boundary conditions, b) your mesh does not extend far out enough (15-30 chords), c) your mesh is not sufficient. All of those can significantly change your results - check a and b first; c likely shows up more for cd and cm. Also, dissipation is a major issue in Fluent - it is very high to keep the solver robust, but it can impact your answers.  Set it as low as possible.

Thank you both for your help and advice.

Maciej, thanks for your description re. Cl and Cd. It makes a lot more sense now.

Marilyn, 

I am using the attached mesh with inlet, outlet, upper and lower surfaces at 50 chord lengths away. For the the boundary conditions, I am using the following: Inlet = velocity inlet, Outlet = pressure outlet, upper and lower surface = symmetry and airfoil = wall. 

Do these seem reasonable? I think they are all okay except the outlet. Should I use an "outflow" for the outlet instead?

I've looked at the tutorial at http://imechanica.org/files/fluent_13.0_workshop02-airfoil.pdf and I can't see anything major that I am doing wrong. I will lower the dissipation and hopefully that helps.

Thanks again,

Aidan

The outlet BC is incorrect - that is used only for internal flows.  Use a Riemann boundary condition -- I assume that's the BC called "outlet".

Marilyn, 

Thank you very much for your help, I really appreciate it. 

I assume when you say to use a Riemann boundary condition for the outlet, you mean "Pressure Far-Field". I tried this, but Fluent says that I need to use and ideal gas. When I changed my fluid properties to an ideal gas (to see what happened), I get divergence in the temperature field (which is not of primary interest to me anyway). I am actually using air, so is there any Riemann boundary condition you could suggest for my example?

Thanks again, 

Aidan

Yes, pressure far-field.  What's the problem with an ideal gas?  If you are trying to match Abbott and von Doenhoff incompressible data in air, ideal gas assumptions are fine.  I'm not sure why your temperature field is diverging.  For incompressible conditions, Fluent may require the "Outflow" condition.  I don't know enough about your problem to provide more guidance.

Thanks Marilyn.

Unfortunately, whilst I have modified the boundary conditions, I have still been unable to increase my Cl value to anywhere near the Abbott and von Doenhoff data. I will keep plugging away at it and will hopefully resolve 

Hi, Aidan,

Just some thoughts on your problem. You may try the following things:

1) Check your mesh quality, especially the orthogonal quality and skewness quality.

2) Check your y+ and turbulence model to see if they match together. I normally use k-w sst with a y+ of 1. Then, you need to ensure the first cell height around your profile. Use this link to calculate your cell height. http://www.cfd-online.com/Tools/yplus.php 

3) I think it is OK to use pressure outlet. You may try to set your upper and lower surface as velocity inlet as well, i.e. no symmetry. 

Good luck.

Regards,

Thanks for that Jialun,

Regarding the quality of my mesh, I have tried to improve this, by reducing the ratio between the smallest and largest cell and by smoothing the mesh. However, is there anything else that I can do? I only know the basics of ICEM so was hoping there was a button which automatically improves mesh quality, similar to the smoothing technique.

Many of the papers I have read suggest the Realizable k-e. In terms of y+ value, I have done a bit of research. As I am using a high Re number (6million, air free stream velocity of 87.64m/s), it is suggested that I use a y+ between 30 and 300. A y+ value of 1 is more applicable to a low-Re number. Therefore, I used y+=30, resulting in an initial cell height of 1.3e-4. Does this seem reasonable?

Marilyn,

I adjusted my BCs based on your comments, so that the upper surface, lower surface and outlet are all pressure far-fields. For 17,000 nodes, I achieved a value very close to the required results, so thank you very much for your guidance. When I increased the number of nodes to 25,000, the Cl and Cd values start oscillating (with a mean of approximately the value I expected) and the residuals also oscillate. I am still trying to resolve this as I'm currently unsure why this is happening.

Aidan

Hi, Aidan, 

You may change the growth rate from 1.2 (default) to 1.1 or 1.05. I commonly use 1.1. The Realizable k-e is also fine. Then, the y+ depends on the choice of wall functions. For Enhanced Wall Functions, you may still need y+ around 1. For your case, I may suggest Non-Equilibrium Wall functions, you can set y+ between 30 and 300. I normally use a y+ of 50 and it works fine..

Regards,

Thanks Jialun, I modified my growth rate, but unfortunately, my values are still oscillating wildly when I used a mesh containing mode than 17000 nodes. For example, the attached is the graph I achieved for 54000 nodes. (Note: "oscillating1" shows just the first 150 iterations, whereas "oscillating" shows over 50000 iterations).

Hi, Aidan,

How did you set the angle of attack? Did you change the geometry (rotate the profile) or define the inlet velocity vector? If you define the inlet velocity vector, I think you have to use the velocity-inlet condition for your upper and lower surface. If you change the geometry, then symmetry or wall is OK. You may give a try.

You can also look this video. It can be helpful.

https://www.youtube.com/watch?v=3VuZiDIl704

Hi Jialun, Apologies for the delay in responding. As I changed the angle of attack, you are right - I changed my upper and lower surface boundary conditions to velocity inlet and I achieved the correct answer. Thanks for the video. I had seen that before, and it was extremely helpful. Also, I found a tutorial on the ansys customer portal which was a great guide to solve my problem using a density based method. I used this tutorial as a guide to solve for the pressure based method, and my answers are exactly as I expected, and in line with published data. Thanks for all your help,

Aidan