[HHK]

Hi all,

I am trying predict the cd, cl and cm of 2D airfoil (NACA0012) with sharp trailing edge and to compare with this technical report. While cl gives excellent agreement (less than 1%), cd and cm shows large deviation (my best was 25%). Please note that I went through previous threads related to this and though there were good suggestions, none worked for me. I am sharing a few snaps and set up info.
Set up info:
1. Structured meshing in ICEM CFD, y+ almost close to 1 with 200k~250k cells.
2. Steady, coupled solver, pseudo transient
3. SA or k-omega SST turbulence model
4. Air (Ideal gas, Sutherland's law of viscosity)
5. Static pressure is adjusted to meet Re = 5.97E6 and Ma = 0.15
6. Far field boundary at 100 times chord distance away.
7. Reference area = 1* chord
8. Components were resolved to set AoA and force report definitions
9. Tried FMG initialization

Please share your thoughts. It would be a great help as I working on project with a time frame.

[amod_kumar]

The reference area for Cd and CL should not be same. I think the reference area for Cd should be 1 [m] x maximum thickness of airfoil.

Regards,
Amod

[HHK]

Originally Posted by amod_kumar

The reference area for Cd and CL should not be same. I think the reference area for Cd should be 1 [m] x maximum thickness of airfoil.

Hi Amod,

Thanks for the reply.
But there is only one reference area option in Fluent.
Is there any reason for this?
Please let me know.

[blackmask]

The reference area for Cd and Cl **should** be the same. A deviation of 25% in Cd is a bit too much. A deviation of 10% in Cd from experimental data should be acceptable for angles of attack below that of stall. You might consider adapt the topology of your mesh and/or make the grid transition between neighboring blocks smooth. The mesh is unnecessary dense in the upstream part of the flow field. If you are doing a 2D calculation, 200k~250k cells is more than necessary (provided that the mesh have a reasonable topology and proper grid distribution). You can make a series of coarser grid to verify the grid independence.

[HHK]

Originally Posted by blackmask

The reference area for Cd and Cl **should** be the same. A deviation of 25% in Cd is a bit too much. A deviation of 10% in Cd from experimental data should be acceptable for angles of attack below that of stall. You might consider adapt the topology of your mesh and/or make the grid transition between neighboring blocks smooth. The mesh is unnecessary dense in the upstream part of the flow field. If you are doing a 2D calculation, 200k~250k cells is more than necessary (provided that the mesh have a reasonable topology and proper grid distribution). You can make a series of coarser grid to verify the grid independence.

Hi blackmask,

Thanks for the suggestions. I will surely check them and update.
Meanwhile, I was going through the suggestions by Langley Research center on running similar cases.

[HHK]

Hi blackmask and Amod,

Now I am okay with low angle of attacks (~4.18 deg) but at higher angle of attacks (~12.25 deg, with same case file), it deviates.
Do you guys have any suggestions?

[blackmask]

It is expected. If you plot the curve you will find that the stall angle given by CFD predications might not agree well with the experiments. The CFD predication near stall angle is less convincing. You might consider to use the drag polar, i.e. , to do the comparison.

[HHK]

Originally Posted by blackmask

It is expected. If you plot the curve you will find that the stall angle given by CFD predications might not agree well with the experiments. The CFD predication near stall angle is less convincing. You might consider to use the drag polar, i.e. , to do the comparison.

Hi blackmask,

I understand that cd prediction at high angle of attack is difficult.
The AoA which I am doing now (~12.25deg) is below stall angle (Please see the curves in this site. I wish to have a CFD prediction of cd at this AoA. I already tried transient analysis for the same mesh (which was okay for low AoA). It didn't work.
Is it fine to use same mesh for high AoA?
Do I need to take care of any other non-dimensional number? (like Strouhal)
Please give me some comments.

[blackmask]

You might want to ensure that the wake region are resolved by sufficient fine meshes. So at high angle of attack you might need to slightly adjust the wake region a bit so that the wake are flow in the fine mesh region. If unsteady vortex shedding is inevitable then time step size should be chosen such that there are at least 10~20 time steps in a period. If you can obtain a converged result with steady calculation, there is no reason that a transient analysis will give a quite different result.

[HHK]

Originally Posted by blackmask

You might want to ensure that the wake region are resolved by sufficient fine meshes. So at high angle of attack you might need to slightly adjust the wake region a bit so that the wake are flow in the fine mesh region. If unsteady vortex shedding is inevitable then time step size should be chosen such that there are at least 10~20 time steps in a period. If you can obtain a converged result with steady calculation, there is no reason that a transient analysis will give a quite different result.

Hi blackmask,

Sorry for the delay in replying.
I made a few changes in the mesh and used k-omega SST with low Re correction checked. Now I am getting reasonable agreement with experimental results up to ~10 deg (at steady state conditions).
Thanks a lot for your help