[frossi]

Hi all,

I am simulating low speed flow over a 2D airfoil NACA 0012 in FLUENT. I can't get my simulation to converge.

My residuals plot and lift plot continue to diverge even after 10,000 iterations (drag plot looks fine). I thought I have a pretty good mesh so I am not understanding what is the issue.

I was thinking that the divergence might be due to the vortexes toward the trailing edge of the airfoil (see attached pictures) combined with the fact that I choose steady state simulation instead of transient. This said, I am not exactly sure why the vortexes are generated in the first place, since my flow speed is relatively low (29.21 m/s), I expect it to be laminar, and I am using a symmetric airfoil (NACA 0012) at 0 deg angle of attack. All these factors together led me to believe that a steady state run was ideal for my case since no time related phenomena such as vortexes was going to arise.

- My questions are:
1) Are the vortexes shown in my pictures a correct physical phenomena for my simulation setup, or they should not originate in the first place given my setup?
2) Are the vortexes combined with my steady state setup the reason why my simulation is diverging? Or there are other reasons?
2) Should I run a transient simulation instead? If so, can I go with pseudo-transient? (I don't understand the difference between the two).

See below they key information for my mesh and physics set up:

MESH
- Structured mesh (see attached pictures for details).
- 205,476 elements (all quads since it is a structured mesh)

FLUENT PHYSICS
- Pressure based solver
- Steady state simulation (it is NOT pseudo-transient)
- Laminar model (since my airfoil chord is 25 cm the Re is < 500,000
- Air with constant density
- Velocity Inlet BC (29.21 m/s)
- 0 deg angle of attack
- 0.5 flow Courant number
- Walls BC for top and bottom domain surface
- Pressure outlet for the back of the domain
- 10,000 iterations conducted

Any help is greatly appreciated!
Thank you guys

[frossi]

I wasn't able to attach the pictures from the CFD POST in the previous message, so I attached them here. Note the vortexes generated toward the trailing edge of the airfoil.

[arnie333]

Hi Frossi,

I cannot see a close-up of your mesh near the airfoil...Did you check element qualities like "Skewness", "Orthogonality" and "Aspect ratio ?

Further, assuming you are using the FLUENT default values for Air Viscosity and Air Density (i.e. sea level ATM conditions), your Re is roughly ~500000. This is on the edge of Turbulent flow, so I would suggest using a Turbulence Solver (perhaps k-w SST) and leave "Pseudo Transient" enabled.

PS. You can also make the top and bottom wall as Slip Wall (No Shear), although this is more for aesthetics.

[hiep.nguyentrong]

can you set min-max distane of your Cd plot close to your magnitude then post here

[frossi]

Arnie,

Thank you very much for your suggestion.
Sorry for the late reply. I conducted a lot of tests during this time.

I tried the k-omega SST model as you suggested and I am getting a solution converged to 1e-09, which I think it's excellent! Do you have some literature that you would recommend reading regarding turbulence models? I would like to be able to justify my choice for this turbulence model.

See below the detailed pictures of the mesh as you asked. I think the mesh looks good. What are your thoughts? Feel free to say if you think improvements are needed.


Now that I was able to solve this first issue, I have these questions:

1) I have a curiosity regarding the residuals plots. For CONTINUITY (black line) and some other residuals, you can see a slight oscillating behavior before the plot flat-lined (see pics). I can't understand what that might mean. In this specific case, I used a mesh with a quite large domain size. With this large domain size, the oscillatory behavior is small, and it dissipates when it flat-lines. When I use a mesh with a smaller domain size, the oscillation is very large, and the residual never flat-lines, as it keeps oscillating, and sometimes it also ends up diverging.

2) I am analyzing the Y plus for this simulation, to determine if it is in the correct range or not. However, I am not sure how to determine this. For my simulation, the Y plus is between 5 and 20 for most of the chord length (see chart). I was reading a lot about this, but people have very different opinions, some saying it needs to be between 1 and 5, some say above 5, some say below 200, etc... . From what I understand (correct me if I am wrong) the Y plus choice varies depending on the turbulence model I choose. I am not sure what would be a way to define if the Y plus range I obtain is good for my simulation or not.

3) For what concerns your last comment you made about making the wall no shear, how would you do it? I don't see an option for that. The only thing I can think of is selecting "specified shear" and inputting 0 for both X shear and Y shear. Is this what you mean?



Thank you for your support.

[frossi]

Nguyen,

Thank you for your reply. As you can read above, I was able to get the solution to converge, so my Cd plot now is fully converged (I don't have a picture to upload here at the moment, I would need to re-run the simulation to take a new screenshot).

However, while I obtain a drag force value of 1.75 N (which I believe to be reasonable for my set up) I get a Cd of 2.3, which seems very high. if i calculate Cd from the lift formula, I get 0.012 for Cd, which is way lower than 2.3. Do you know why Fluent is outputting such a high value? I suspect it has to do with the reference values (see pic)? or some other information I input during set up?

Thank you!

[hiep.nguyentrong]

Originally Posted by frossi

Nguyen,

Thank you for your reply. As you can read above, I was able to get the solution to converge, so my Cd plot now is fully converged (I don't have a picture to upload here at the moment, I would need to re-run the simulation to take a new screenshot).

However, while I obtain a drag force value of 1.75 N (which I believe to be reasonable for my set up) I get a Cd of 2.3, which seems very high. if i calculate Cd from the lift formula, I get 0.012 for Cd, which is way lower than 2.3. Do you know why Fluent is outputting such a high value? I suspect it has to do with the reference values (see pic)? or some other information I input during set up?

Thank you!

u must set ref value to calculate cd (velocity, area, length, rho) or report drag and calculate it

[diogoncsa]

Originally Posted by hiep.nguyentrong

u must set ref value to calculate cd (velocity, area, length, rho) or report drag and calculate it

What are the ref values for this case? I am having the same low cd and cl issue with airfoil 2D simulations

[hiep.nguyentrong]

velocity: 29.21 m/s, length : 0.25, area: 0.25

[diogoncsa]

Originally Posted by hiep.nguyentrong

velocity: 29.21 m/s, length : 0.25, area: 0.25

That solved my problem, thanks Nguyen!

[AidealZohary]

Hi, this is an old thread. But if anyone is still interested to run a simulation on the NACA 0012, NACA 4415, FX 61-184 E420 and S1223 airfoil, please take a look at:

Numerical Investigation on the Pressure Drag of Some Low-Speed Airfoils for UAV Application.

https://doi.org/10.37934/cfdl.13.2.2948

Unsteady 3-equation k omega intermittency SST was used. Good comparison with XFOIL and experimental data. Transition features also shown through cf and cp plots.

Learn how I designed the mesh here:

https://www.youtube.com/watch?v=qZRqBu9Ss2U