Some update: - I understand y
 

Some update:
- I understand your bc now. this looks fine
- GAMG looks better but I am still unhappy with pressure convergence
- How do you initialise Fluent?
- Do you run fmg-init in Fluent?
- What do Fluent residuals look like?

Regards

Good morning FOAMers! @ Bas
 

Good morning FOAMers!

@ BastiL

1) Ok, perfect! In any case... My boundary conditions are:
- patch named ext: v (15, 0, 0), p zeroGradient, k = 0.001, epsilon = 0.000616218, that is the same of an inlet (v (15, 0, 0) is only an example)
- wall named surf: v (0,0,0), p, k, epsilon zeroGradient,
- patch named symmetry.5: v, p, k, epsilon symmetryPlane,
- internalField: v (15, 0, 0), p = 0, k = 0.001, epsilon = 0.000616218
These settings are in agreement with Fluent BC.

2) Ok!

3) I initialized Fluent from the "ext" BC: Solve → Initialize → Compute form "Ext". That's why I set internalField equal to ext in my bc.

4) What do you mean with "fmg-init"? Can you be more precise?

5) See attached file for my residual history.

6) About prism layers... A good quality prism layer for such a wing is difficult to obtain with Gambit 2.3. Moreover, at the moment I am more concerned about describing flow separation in a meaningfull way. In any case, I will give a try with a new mesh and with nOrthogonalCorrectors 0.

@ Daniel
Sure you can! You will get it soon.

Cheers, Maddalena

Always problems in attaching f
 

Always problems in attaching files...
http://www.cfd-online.com/OpenFOAM_D...s/mime_pdf.gif residualHistory.pdf

Time = 9 DILUPBiCG: Solvin
 

Time = 9

DILUPBiCG: Solving for Ux, Initial residual = 0.0047906, Final residual = 3.78068e-07, No Iterations 5
DILUPBiCG: Solving for Uy, Initial residual = 0.00373367, Final residual = 7.91143e-07, No Iterations 4
DILUPBiCG: Solving for Uz, Initial residual = 0.000911481, Final residual = 1.92399e-07, No Iterations 4
GAMG: Solving for p, Initial residual = 0.489951, Final residual = 9.58598e-07, No Iterations 18
time step continuity errors : sum local = 8.22587e-08, global = -1.34617e-16, cumulative = -1.01119e-15
DILUPBiCG: Solving for epsilon, Initial residual = 0.000357599, Final residual = 9.27643e-07, No Iterations 5
bounding epsilon, min: -0.0638691 max: 19992.8 average: 109.875
DILUPBiCG: Solving for k, Initial residual = 0.000366048, Final residual = 6.30599e-07, No Iterations 6
bounding k, min: -0.000336714 max: 17.7073 average: 0.36009
ExecutionTime = 179.32 s ClockTime = 181 s

Thats how a typical iteration output looks for me. I can run several hundred iterations without problems but I am unhappy with pressure convergence so far. Your mesh is much too nice for any non-orthogonal correctors. Look at the errors - its good. I need some more time for fine-tuning but in generall i would do:

p GAMG
{
agglomerator faceAreaPair;
smoother GaussSeidel;
nCellsInCoarsestLevel 50;
mergeLevels 1;
tolerance 1e-06;
relTol 0;
and:

default Gauss linear;
grad(p) Gauss linear;
grad(U) Gauss linear;

Keep it simple for the beginning. If these settings will run I will go more to detail. However you also used simple settings in Fluent so this should not be too bad.

Regards

Hey, got your mail will get
 

Hey,

got your mail will get to it over the weekend - unfortunately I have to finish something else first - but I have an eye on the thread and will incorporate all changes that will be suggested or discussed.

I will hit you back on Monday

- harly

I run two numerical variants s
 

I run two numerical variants so far. Both are are running 400 Iterations w/o problems but give totally different results. I have to go deeper into it.

The case you sent me is 8°AoA, right?

Regards

I have run some simulations as
 

I have run some simulations as well. I have focused on gradSchemes, since Gauss linear is stable, but force coefficients are not converging. I added a limiter as suggested by Hrvoje at the beginning of this thread, without success. leastSquares scheme gives no stable simulation.

The case I send is with AoA = 24°, since I guess that if I can find a good simulation set up for a stalled wing, I can apply it to any other AoA.

I feel we are getting closer! Let's keep in touch.
Ragards,

Maddalena

Dear BastiL, after a succes
 

Dear BastiL,

after a successfull run with my case, I realized that a spherical domain is not suitable for OF. Why? See this velocity magnitude contour...
http://www.cfd-online.com/OpenFOAM_D...your_image.gif
Nice vortices, uh! Probably simpleFoam needs an inlet and an outlet to define the flow correctly. It seems like that the flow bumps to the upper right domain, at 24° from the horizontal, I guess... I will investigate how and why such vortices generated. These vortices are also the cause to all the problems I had so far, I suppose. However, working in such an extreme condition helped me to understand better how OF works and how set simpleFoam parameters correctly.

In the meantime, I generated a new mesh with a cube domain. I am running a case with the same settings as above, in particular using gaussSchemes equals to faceMDLimited Gauss linear 0.5 and setting k and epsilon values higher than in Fluent to have flow separation. If you like to receive this case as well, just ask!

Thanks for your help so far!
Maddalena.

http://www.cfd-online.com/Ope
 

http://www.cfd-online.com/OpenFOAM_D...s/mime_pdf.gif velocityField.pdf

Well... sounds good. I expe
 

Well...

sounds good. I expected this bc to be difficult in the first moment but after I saw the Fluent residuals I was sure OF should run on it - and I still think it should work.
I would be interested in your second case for some more tries, please. I will do some more over the weekend and get back to you on monday.
What about Fluent results for 24°AoA? How to change the 24° OF-Case to 0° and 4°? Simply changing velocity direction?

Hello, I agree with Bastil.
 

Hello,
I agree with Bastil.
It should work even with spherical domain unless the domain was too small, but in this case you should have had the same problem with Fluent.

It seems there is something wrong with the boundary condition.
Did you set to inletOutlet k and eps BC at the spherical ext patch?

Hi Rosario, I set fixedValue
 

Hi Rosario,
I set fixedValue both for k and epsilon at the spherical ext patch. Should I have used inletOutlet since the flow "runs" in the two directions?
Regards,

Maddalena

Yes. I don't know if this is
 

Yes.
I don't know if this is a big problem, but consider that with inletOutlet BC k and eps are set to zero gradient if the fluid is leaving the domain end set to fixed values if it is going in.
If you choose fixedValue BC you are fixing k and eps in any case, and this may cause some problems.

I think it is worth trying..

Hi Maddalena, I saw you wr
 

Hi Maddalena,

I saw you wrote in a thread I started and asked about if I solved my issue with a steady solver for a transonic case. I'm sorry to tell you that I did not, I ran it transient until I reached convergence. But I'm still struggling with the problem you have here, I'm trying to validate some experimental data and I cant get the correct solution with OpenFOAM. As you also did I ran the same problem in Fluent, there I get a fairly good solution. What I don't understand is why the same case dose not give the same solution in OpenFOAM.

I'll follow this thread and see if anyone comes up with some good ideas..

Mathias

Hi guys, finally I have some
 

Hi guys,
finally I have some good news from my simulations!

1)Thanks to Rosario's suggestion, I changed my boundary condition for the spherical domain from fixedValue to inletOutlet. In simple words a fixedValue inlet applied to the ext patch would eventually do not let the flow goes out of the domain (as it does in Fluent) and flow arriving at the upper-right surface of the sphere is in some way forced to turn back. This is also the reason of the two vortices that you could see on the above .pdf file. Therefore, bc for a wing in a half-sphere domain are as follows:

- sphere surface (patch named ext): U, p, k, epsilon inletOutlet, with inletValue fixed as above: v (15, 0, 0), p = 0, k = 0.001, epsilon = 0.000616218,
- wing surface (wall named surf): U fixedValue (0 0 0), p, k, epsilon zeroGradient,
- symmetry plane (symmetry.5): U, p, k, epsilon symmetryPlane,
- internal domain (internalField), U, p, k, epsilon uniform fields, defined as in ext.

With these values, the simulation runs without stability problems and without any "odd" flow features. Lesson learned: Fluent applies things without saying, OF forces you to use your brain!

2)I had good results from the cube domain as well. In that case, I applied a fixedValue inlet bc as made before, not only to the inlet face, but also to the front, rear, upper and lower patches.

3) In both cases, velocity and pressure contours plots are as they should be for a stalled wing, with a nice detached flow near the trailing edge...

3)Results from 1 and 2 are comparable, even if I haven't obtained forces convergence yet. I guess that it is only a matter of schemes fine tuning. I will try suggestions made up to now, and of course any new suggestions are welcome!

4)Comparison between average OF results and converged Fluent results for an AoA = 24° is as follows:
cl: OF = 0.755, Fluent = 1.012
cd: OF = 0.355, Fluent = 0.401
As you can see, they are pretty close, but I am sure I can do more. As said before, I think I need to refine schemes...

That's all... Nice, uh? I will let you know how the story ends...

Cheers, Maddalena


<u>@BastiL</u>
Yes, change velocity components in 0/U and you'll get every angle of attack. And do not forget to change liftDir and dragDir in system/controlDict for force calculation. ;-)

Thanks Maddalena, I will do
 

Thanks Maddalena,

I will do so. Is it possible to get you second case, please?

Thanks BastiL

Hi, that's great news I am
 

Hi,

that's great news I am still struggling with my sphere - my drag is way to high. I would be interested in your "cube" domain case just to see what dimensions you used and to give it a go for myself.

Thank you very much.

- harly

Hi Maddalena, Did you ever
 

Hi Maddalena,

Did you ever manage to match the data from Fluent with OpenFOAM? I am plotting the pressure coefficient on the upper and lower surface on a 3D wing, the curves match pretty well on the lower surface, but on the upper it does not look good at all. The Mach number is 0.5 so I dont have any shocks that is interfering.

Let me know if you ever manage to get the data to match and if you know why they didn't match earlier.

//Mathias

Hi again, Do you think tha
 

Hi again,

Do you think that you could send me your case? I want to look at it and see if I can get any ideas for future work.

Thanks,

//Mathias

Hi guys, I am still doing som
 

Hi guys,
I am still doing some tests to set everything properly. As soon as I am appy with my case set up, I will post here the comparison results and send it to you.
Bye,

Maddalena.