[MadsR]

Hi.

I get drag overprediction from CFX simulations of an 2D airfoil

Setup info:
1. I have an 2D airfoil setup in CFX
2. Mesh is created in ICEM Hexa. 200k->900k mesh dependent tests done
3. max(y+)<1
4. turbulence model is k-omega-SST
5. fully turbulent, no transition
6. angle of attacks investigated 0-15deg
7. Re is 3e6
8. domain extents sensitivity is investigated, 60chords of domain extent is found sufficient
9. butterfly/O-mesh, inlet (bottom/left)-outlet(top/right) BC's
10. high-resolution and specified blend factor of 1.0 is investigated
11. convergence to 1e-6 (max residuals) and lift/drag convergence monitored

I compare these CFX results with an academic code which has a good track record. I get less than 1% discrepancy on the lift coefficient, which is quite good. But drag (which I know is harder to resolve) is off by up to 20% (more than the academic code).

Any suggestions on what to check? Help would be greatly appreciated.

/Mads

[ghorrocks]

What accuracy did your mesh and boundary proximity tests show?

What turbulence model does the academic code have? What about turbulence inlet conditions? Is a turbulence transition model needed?

[MadsR]

Hi Glenn. Thanks for your feedback. I am in the process of doing formal grid dependence tests but proximity-tests showed that I needed around 60-chord-lengths of extent to get best results. Drag was 40-50% off when using a 40-chord-extent mesh and now down to 20% when using 60-chord-extent. 80-chord-extent doesn't improve anything.

The turbulence model used by the academic code is the same as mine, mentioned above (k-omega-SST). Transition model is needed but this case is run with and without and I am currently testing without and comparing to academic results without transition.

It is my experience that setting a turbulence level does not change solution as it is so far away from the airfoil that it will dissipate way before reaching the airfoil. Do you experience otherwise? Turbulence inlet level is zero in the academic simulations and set to "low" in mine.

Thanks, and please continue to ask such questions, there might be something else I have missed :-)

/Mads

[Bak_Flow]

Hi MadsR,

This is interesting. I did a bunch of cases back about 5 years ago with CFX and found about the same over-prediction. I was doing simple NACA uncambered airfoils ie 0012, 0009, 0012, etc.

At the time the transition models had not been full implimented and the story was that the difference between experiments and predictions were due to the lower skin friction from leading edge to tranition point in the experiments. The other major issue was that stall was predicted late and under-predicted.

I actually found that smaller domains upstream could be used reliably if you are careful about setting k and epsilon at the inlet. As you point out k dies away if you have a finite epsilon at the inlet. What you have to do is ensure that you have turbulent viscosity = 0 or some constant by the time the flow gets to the leading edge. AND be consistient between different domains!

Another thing you have to be careful with for turbulence quantities is that most codes never let k=0 because of divide by zero for terms like (eps/k) which is used in all the linearizations, etc. So each code will have some different arbitrary number. You just have to make sure that you are consistient.

Yet another thing in CFX is that k and epsilon are solved first order by default (since wiggles can produce negative numbers and stability problems....divergence). So you can get some unexpected things happening near the leading edge where k~0 upstream.

I have not revisited these cases which were pretty disappointing for such simple cases ~ 5 years ago! There probably are some new settings, etc to fix things up by now. The interesting lesson from these cases is that you really learn what is important when you apply a code to such a simple geometry. The drag on the airfol(unstalled) is all skin friction....and if you don't get the models set-up right.....look out! A 3-D case with flaps, separation, etc. "hides" some of these details.

What academic code are you using?

Let us know how you make out!

Regards,

Bak_Flow

[MadsR]

Hi Bak_flow and thanks a lot for your valuable input. I can't comment much on the academic code since I am not using it and are referring to to results which have been kindly handed to me by the academic institution. I am sure they don't mind, but you never know.

Nice points about the inlet turbulence and turbulence is still solved by first order numerics in CFX by default. Also zero values causes issues.

At the moment I am following two paths: 1) mesh dependency study with different meshes to observe truncation error and 2) two mesh-domains in ICEM, i.e. one for the near-profile-domain and one for the outer part. They end up being one domain, but in this way I can ensure that the boundary-layer cells do not move when I expand my domain.

I will get back with more results and/or indications later.
/Mads

[ghorrocks]

CFX V12 has high order numerics for the turbulence model as an option. You might need this for your application.

Does the academic code have the SST model? While the basic idea of the SST model is published in the open literature there are lots of under-the-hood bits of it which are proprietary. I don't think the turbulence models will be the same unless you choose something like k-e, and even then you have to be careful about the issues Bak-flow mentions and the order of the turbulence numerics.

[MadsR]

Thanks for your feedback, Glenn :-)

I will look into the second order numerics for turbulence.

SST: Yes, and both results are with SST model. I am also thinking that the academic code might feature some "tuning" of parameters and I have to investigate this further.

Keep posting such valuable info.

/Mads

[MadsR]

Initial experience with high resolution numerics on turbulence is that it won't converge...In my grid dependence study I have three meshes and with highres turbulence numerics I can't get convergence on the coarsest mesh. Actually normally you would convergen more easily on coarse meshes due to the high numerical diffusion, but I guess not when it comes to this case.

/Mads

[ghorrocks]

Of course the high resolution numerics will be harder to converge. Use the results you already have as an initial condition, that should help a lot.

[MadsR]

@Glenn: Well I guess not necessarily so. The "high resolution" in CFX is just a automatic blending function so in theory it should give good convergence. At least that's how it works for the advection numerics. In case of "trouble" it switches to first order, else it is second order central differencing.

Naturally, I started out from a previous simulation with pure upwind on the turbulence terms, and it just doesn't converge. Well, it does converge to in-between 1e-3 - 1-e4 but not in a smooth way as the turbulence-upwind which converges to machine precision in one smooth swoop. Neither does it converge from a complete restart, which makes sense.

/Mads

[ghorrocks]

Have you run through the suggestions here:

http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Now you are resolving the turbulence more accurately you are probably picking up smaller and possibly transient features and these are causing convergence difficulties.

[MadsR]

Hi Glenn. Thanks a lot for that pointer - I will look through it.

I found that changing between zero pressure at the outlet or averaged zero pressure at the outlet changed roboustness (the averaged being the most robust, which seems reasonable).

[Bak_Flow]

Hi Mads,

another option you might look at is setting the blend factor for the turbulence equation discretization yourself.

I am a bit of a doubter and don't always like the code making decisions for me....and in some cases have seen some wierd things going on to back it up....with hi-res!!

You have to play a few tricks since the gui does not have the blend factor option. You can either edit the .ccl yourself and inject it into the def file or you can use the def file editor starting with a .def for hi-res. for turbulence and then adding the appropriate parameters ie switch the parameter for turbulence to specified blend factor and then adding the blend factor you want.

Usually something like 0.9 or 0.95 will give you near second order for convergence of turbulence quantities and should be as robust as hi-res...and you know what you have got!

Let us know how the results look and if you need any more pointers.

Regards,

Bak_Flow

[MadsR]

Hi Bak. I totally agree with you, I also prefer to explicitly specify such figures. Thanks for the info.

/Mads

[Dr. Flow Squad]

Hi Mads.
What was the outcome of this? Still difficult drag predictions?

[MadsR]

Hello Dr Flow Squad :-)

Well, I am still trying and now I tested for sensitivity of y+. I have varied max(y+) from 0.23 to 4.2. Quite expected as long as max(y+)<2, Cl does not vary much (about 0.5%) but when max(y+) get above 2 I get a difference of 5-10%. Also as expected.
For Cd, the value changes around 2-3% when max(y+) varies below 2 and by 20% when max(y+) goes up to 4.

It seems that max(y+)<2 is okay. Nothing new here, I know, but I just did the check with CFX and the SST model.

/Mads

[HHK]

Originally Posted by MadsR

Hello Dr Flow Squad :-)
For Cd, the value changes around 2-3% when max(y+) varies below 2 and by 20% when max(y+) goes up to 4.
/Mads

Hi Mads,

Can you please tell me how were able to reach cd variation close to 2% ?
I have read the entire thread. I am also facing the same issue (in Fluent though).
What was the critical point which helped you? Please make your comments.

[ghorrocks]

There is no single thing you need to get right for accurate simulations. There is a whole bunch of things which need to be correct to get accurate results. Have a read of the FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

[HHK]

Originally Posted by ghorrocks

There is no single thing you need to get right for accurate simulations. There is a whole bunch of things which need to be correct to get accurate results. Have a read of the FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

Hi Glenn,

Thanks for the reply. Recently, I posted a similar question on Fluent forum. I am facing same situation which Mads faced a few years ago. The cd and cm values are getting over-predicted while cl is in good agreement. I wish to know what was the main change he made in his simulations which got him good prediction of cd (viz. lower y+, more number of cells on airfoil surface, turbulence model).

I am sorry to continue this old thread as I can not start a new one in CFX forum since I use Fluent.

[ghorrocks]

In general, for an airfoil in attached flow getting CL accurate is pretty easy. The inviscid result will give you CL reasonably well, so things like turbulence model, transition and so on are not very important. CD and CM require an accurate boundary layer model and that requires accurate turbulence modelling - so getting CD and CM accurate is much more challenging.

So consider your turbulence model, whether you need to model transition, mesh resolution (both normal and along the chord) and mesh expansion ratio. And that is just a few parameters which come to mind, there is much more to consider beyond that.