[mingersai]

Dear Friends

I'm running simulation on a NACA 64 210 airfoil with k-omega sst model with Re = 2.6 E6 . The chord length is 1m.

Angle of Attack ranges from 0 to 20. I'm changing the inlet velocity for different angles. Mesh is shown below


everything is fine before angle of attack getting to 12 degree, both lift coefficient and drag coefficients oscillates periodicly after 12 degree



I don't know if this is the correct solution. However, before this angle the results are reasonable

Is it because of the mesh? Does it mean changing inlet velocity is not correct for higher degree angles of attack?

Thanks for your help.

[cfdnewbie]

Hi,
I'm no expert on steady calculations, but I would guess that with increasing AOA, your problem becomes ever more "transient", since (in reality) you would see serious vortices rolling up from the nose and shedding with some characteristic frequency....

So I guess that a steady approximation of this unsteady problem has reached its limits, and the RANS has problems converging to a steady state.

Hope this helps, maybe the RANS guys here could confirm / refute?

Cheers

[mingersai]

Originally Posted by cfdnewbie

Hi,
I'm no expert on steady calculations, but I would guess that with increasing AOA, your problem becomes ever more "transient", since (in reality) you would see serious vortices rolling up from the nose and shedding with some characteristic frequency....

So I guess that a steady approximation of this unsteady problem has reached its limits, and the RANS has problems converging to a steady state.

Hope this helps, maybe the RANS guys here could confirm / refute?

Cheers

Hi, Thanks for replying~ Does it mean this simulation result is reasonable? I found some experiment results for this angle of attack, I'm not sure how experiment people pick up the values for lift and drag if vortex shedding etc. is happening...
I have no experiences in wind tunnel tests at all. Hope some experts could help me out

[Martin Hegedus]

Are you using local or global time stepping? Is your grid structured or unstructured? If you are using local time stepping with a structured grid and the grid cells become small compared to others in the near vicinity (such as one finds at the trailing edge), you'll get a spatial variation of time step which could also cause the flow to go unstable. The small structured grid cells create a blockage.

[cfdnewbie]

Adding to the points mentioned by Martin: Explicit or implicit time stepping? if you are doing RANS, I'd guess implicit....if so, check your CFL, maybe your steady solver actually starts to pick up unsteadiness....

[mingersai]

Thanks for all your replies.
I'm using unstructured mesh, and transient formulation is implicit.

I had changed to run for steady state solution, I got converged solution


I'm not sure why transient solution would oscillate....

[cfdnewbie]

Originally Posted by mingersai

I'm not sure why transient solution would oscillate....

Well, if the flow separates periodically or periodic vortices form, then of course your lift and drag would show the same behaviour.... so maybe I am misunderstanding your question??

[mingersai]

Originally Posted by cfdnewbie

Well, if the flow separates periodically or periodic vortices form, then of course your lift and drag would show the same behaviour.... so maybe I am misunderstanding your question??

Thanks~

I should read more about airfoil stalling... I don't really understand how experimental people measure Lift and Drag at this angle.... I found some experimental results for comparison and they only show a single value for this.

Can you recommend me some book talks about lift and drag measurement at stalling angles?

[sail]

High AoA foils Cl is avaraged in the wind tunnel over a certain time. this is to have a sinlge meaniningful result of a phenomenon wich is unsteady.

More specifically, a stalled foil will be charachterized by grat separation, setachment and consequently vortex generation in the wake.

While a steady RANSE will converge to a certain value, it will probaly be wrong. Not only a numerical avaraging will loose and/or smear lot of high intensity phenomenon, but usually ranse turbulence models will not be able to predict accurately the detachemnt and the other physics that take place.

if you need some meaningful results, I would recomand to switch to LES symulations.

https://www.youtube.com/watch?v=J-xxCkebdZs here you can see exactely what happens in the stall and pre stall phase.

[mingersai]

Originally Posted by sail

High AoA foils Cl is avaraged in the wind tunnel over a certain time. this is to have a sinlge meaniningful result of a phenomenon wich is unsteady.

More specifically, a stalled foil will be charachterized by grat separation, setachment and consequently vortex generation in the wake.

While a steady RANSE will converge to a certain value, it will probaly be wrong. Not only a numerical avaraging will loose and/or smear lot of high intensity phenomenon, but usually ranse turbulence models will not be able to predict accurately the detachemnt and the other physics that take place.

if you need some meaningful results, I would recomand to switch to LES symulations.

https://www.youtube.com/watch?v=J-xxCkebdZs here you can see exactely what happens in the stall and pre stall phase.

Thank you very much ! It's very helpful~!

[Martin Hegedus]

In the beginning Ming mentions that his Re is 2.6e6. His RANS solutions, even up to 20 degrees, are probably OK, everything considered. LES will be expensive. And, I wouldn't necessarily trust the WT results passed stall either. The side walls can affect the results.

[sail]

Originally Posted by Martin Hegedus

In the beginning Ming mentions that his Re is 2.6e6. His RANS solutions, even up to 20 degrees, are probably OK, everything considered. LES will be expensive. And, I wouldn't necessarily trust the WT results passed stall either. The side walls can affect the results.

While I agree that experimental testing might have some source of error, maybe ever more "dangerous" that cfd because there are no benchmarks to measure aganist, i have never been able to get accurate results on stalled foils at a regimen between re 2e5 and 2e6 with RANSE. (I'm investigating mostly symmetrical, monoelement foils, so around 10-14° is how much i can go with confidence).

While i'm just starting to "play" with LES, i agree that it is expansive, even if i've seen quite good results even using wall functions or DES. It all depends on the pourpuse of the analysis, maybe some tradeoffs are necessary accomplish the goal.

[Martin Hegedus]

Originally Posted by sail

While I agree that experimental testing might have some source of error, maybe ever more "dangerous" that cfd because there are no benchmarks to measure aganist, i have never been able to get accurate results on stalled foils at a regimen between re 2e5 and 2e6 with RANSE. (I'm investigating mostly symmetrical, monoelement foils, so around 10-14° is how much i can go with confidence).

While i'm just starting to "play" with LES, i agree that it is expansive, even if i've seen quite good results even using wall functions or DES. It all depends on the pourpuse of the analysis, maybe some tradeoffs are necessary accomplish the goal.

Well, I don't think, in general, I'm going to say I have confidence in any of this. Only after I know a lot more do I start feeling comfortable.

What follows is my impression only.

Overall, when done right for an airfoil, I feel LES is better than RANS, ignoring the time penalty. In general, i.e. arm waving, when Re gets below 1e6-2e6 I do start feeling uncomfortable with RANS. Above this, LES and RANS start approaching one another for tripped results. From what I understand, neither do well for transition (i.e. drag buckets) unless the turbulence models get tweaked. But there is a lot of research in this area and I do not claim to be up to date.

Then there is the wind tunnel results. One needs to be careful that the walls above and below the airfoil are far away. Unfortunately I don't have a rule of thumb. But I would say at a minimum 10 times the chord. In general you will not find that. I've seen CFD results miss the cl lift curve slightly and claim it is the turbulence model. The turbulence model gets switched, usually SA to SST, better agreement is obtained, and success is claimed. But if one models the walls, they may find that the SA is better. Then there is separation. Usually the airfoil is mounted on a turn table or splitter plate. This, along with any upstream BL which is influencing the results, is enough to cause the the airfoil sides to stall first. This tends to delay stall at the center section where the pressure taps and rake are.

In regards to RANS, it is nice to seen when people model the WT. Or at least just a box around the airfoil. For values before stall it is OK to give the walls a slip condition. Then one does not need to worry about boundary layers. Then do like the experiment. Calculate lift by integrating the pressure and calculate drag by using a rake. If you calculate drag by integrating the surface values, you'll find that the answer may be off if the WT walls are affecting the results. The reason is that the rakes do not go far enough to capture wall effects. In regards to the region of stall, I don't have best practices in regards to modeling the WT wall boundary layer. But something is nice. Maybe best and worst cases.

[mingersai]

Thanks for your guys discussion~ I learnt a lot from this ~