Hi FOAMers, I'd like to com
 

Hi FOAMers,

I'd like to compare Fluent 6.3 and OF 1.5 performances in simulating flow around fixed wing with a Reynolds number of about 220000. In both cases, I applied to simpleFoam this tetrahedral mesh:

[...]
Number of cells of each type: [...]
tetrahedra: 445207 [...]
Checking geometry...
Overall domain bounding box (-1.865 -4.09798 -4.09726) (6.335 9.22699e-09 4.09726)
Mesh (non-empty) directions (1 1 1)
Mesh (non-empty, non-wedge) dimensions 3
Boundary openness (1.52724e-19 7.40957e-19 2.03325e-19) OK.
Max cell openness = 1.63569e-16 OK.
Max aspect ratio = 9.33635 OK.
Minumum face area = 5.21732e-07. Maximum face area = 0.156288. Face area magnitudes OK.
Min volume = 3.97085e-10. Max volume = 0.0188268. Total volume = 144.059. Cell volumes OK.
Mesh non-orthogonality Max: 65.4365 average: 20.2284
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.899635 OK.

the following fvSchemes:

[...]
divSchemes
{
default none;
div(phi,U) Gauss upwind;
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div(phi,R) Gauss upwind;
div(R) Gauss linear;
div(phi,nuTilda) Gauss upwind;
div((nuEff*dev(grad(U).T()))) Gauss linear;
[...]

and fvSolutions:

[...]
relaxationFactors
{
p 0.3;
U 0.7;
k 0.8;
epsilon 0.8;
R 0.7;
nuTilda 1.0;

Not specified parameters are as standard. Boundary conditions are as follows:

- inlet: velocityInlet, v (15, 0, 0), p zeroGradient, k = 0.001, epsilon = 0.000616218,
- wall: v (0,0,0), p, k and epsilon zeroGradient,
- symmetry plane for the central plane,
- internalField: v (15, 0, 0), p = 0, k = 0.001, epsilon = 0.0616218 (two order of magnitude greater than the inlet, as suggested here).

Note that there is not an outlet since the entire domain is shaped as a half-sphere with the wing placed somewhere at about 1/3 of the diameter. In addition, I added wall roughness to wall functions, as explained here, and set kappa = 0,4187, E = 9,793, C_s = 0,5 and k_s = 0,0004.

I run the simulation for an angle of attack of 0° and 8°. These are my results:

AoA = 0°
- OF 1.5: cl = 0.0332, cd = 0.020838;
- Fluent 6.3: cl = 0.0406, cd = 0.0480.

AoA = 8°
- OF 1.5: cl = 0.268883, cd = 0.0.04841;
- Fluent 6.3: cl = 0.6317, cd = 0.08704.

As you can see, there is a difference of about 50% in both cl and cd, at both AoA values. In addition to these, I ran a simulation with AoA = 24° and, while in Fluent I obtained a complete stalled wing as expected, I had no sign of flow detachment in OF.

So far, I have tried different solutions and configurations, including:
1) change external domain shape from a sphere to a cube (inlet condition as above, outlet condition: p = 0, v, epsilon and k = zeroGradient);
2) increase cell number;
3) take the flow as laminar;
4) change epsilon and k relaxation factor to 0.3;
but anything is worth mentioning.

Is there anything that I am missing? Some bad assumptions? And... is there anyone that have a sort of "general rules" for this kind of problems?
Any help will be appreciated.
Regards,
Maddalena.

Hello Maddalena,
 

Hello Maddalena,
Iam new to OPENFOAM but i can suggest some basic guidelines for such stalled wing profile computations..

1. Under stall regions wall functions are not recommended. So you need to capture the near wall turbulence shear and seperation point accurately. You should have Y+ around 1 and try it with low Re model. Launder Sharma ke model or others..

2. It seems all High RE model in OPENFOAM only uses wall function. If you are using Wall function then make sure that the first cell center from wall should be placed at around 20 to 30 Ref. ERCOFTAC (1999).

3. Inregards with grid i hope you might have some fine Boundary layers at near wall regions. If not its essential.

If you have followed all these things then i donot know.... Lets wait for some other Foamers who experienced such flows..

Regards

Maddalena, I agree on Marut
 

Maddalena,

I agree on Maruthamuthu points. Additionally I strongly recomend to change the divScheme for the convective term of the momentum-equation:

divSchemes
{
...
div(phi,U) Gauss upwind;
...
}

You are presently using first order upwind which introduced a lot of numerical diffusion. Try a second order scheme.

Secondly (depending on your domain size) the inlet turbulence can affect the results. Try to find out the exact setting used in your fluent computation an apply them in Foam.

And last point: which turbulences model are you using (in Fluent and in Foam)? And is there a correction for the stagnation point (e.g. Kato-Launder) activated?

If you like, you can email me your case, than I can have a closer look.

Dear Maruthamuthu, Dear Daniel
 

Dear Maruthamuthu, Dear Daniel,

thanks for your support and advices. Here there are some answers (and some more questions as well...):

1) I have some problems to apply Fluent boundary condition for turbolence exactly. In fact, if I use converged Fluent value for k and epsilon both in boundaries and in internalField, my simulation does not converge, in the meaning that cl and cd values oscillate giving meaningless results (negative cl, for example). The main reason for that is that epsilon value is not sufficiently uniform within the domain and has to be bounded by simpleFoam. Using the trick of an epsilon two order of magnitude lower within the domain let the simulation converge.

2) At the moment, I am using realizableKE model for turbolence, both in OF and in Fluent, with the same (the defalut) realizableKECoeffs. There is not any stagnation correction modelled in it.

3) I am running a Hi-Re model, and my yPlusRAS -latestTime check says that: […] Patch 3 named surf y+: min: 0.322683 max: 13.9875 average: 2.08982. In any case, I remeshed my domain to obtain a grid with a max y+ around 25, the simulation is running... stay tuned for updates!

4) I know that low-Re models should be applied when the turbolent Reynolds number is low enough and viscous effects are important. However, I am wondering if there is a sort of correlation between the turbolent Reynolds number and the flow Reynolds number, i.e.: in which Re range should I use a Hi-Re model or a Low-Re model? In any case, I have some doubts that a low-Re model is the right one for my case, since the what I'd like to simulate is not only stall and post stall, but also the behaviour with low AoA, with no flow separation.

5) Of course, I can see a small boundary layer around my wing...

6) And... I changed my div(phi,U) to div(phi,U) Gauss linear. Thanks.

After a closer comparison of p, U, k and epsilon countour plot obtained with OF and Fluent converged simulations, I can add that:

1) p max and min values are not the same in OF and Fluent, however the data range (pmax – pmin) are almost the same.

2) U range are the same.

3) Epsilon and k values are way too low in the OF converged solution, and I think this is the main reason of my low aerodynamic coefficients. Maybe the above trick helps to let the solution converge, but towards wrong values...

However, I am not puzzled by numerical values... well... not only from them. I think that the most strange result is an attached flow for such a high AoA as 24°. I agree that the turbolence model could be not the right one for this kind of problem, but... I expect that the flow separates in any case! Is this strictly connected with my low k and epsilon values? Or maybe should I change my solver e.g. turn to turbFoam?

Cheers,

Maddalena.

... about point 3: the simulat
 

... about point 3: the simulation yith a y+ of about 25 blew in 50 iterations. As usual, epsilon range became way too large and has to be bounded by simpleFoam. This happened although a higher epsilon was applied in the domain in comparison of innerField epsilon.

At this point, seems to me that the problem is strictly connected with starting epsilon value. Is there any way to have a good estimation of it a part using Fluent converged value (that does not work...)?

Regards,

Maddalena

Back to basics: - run checkMe
 

Back to basics:
- run checkMesh, and check non-orthogonality
- you cannot run central differencing on div(phi,U): choose an NVD or TVD scheme
- you probably need to switch on some limiters (in Fluent, they are on all the time):
grad scheme: faceLimited leastSquares 0.5;
laplacian scheme: Gauss harmonic limited 0.5;

This is probably enough to sort out your discretisation and you will get a decent solution. Don't forget to declare the surface of the airfoil as a wall patch (wall functions!)

Enjoy,

Hrv

Hello Maddalena,
 

Hello Maddalena,
Follow the steps in regards with mesh quality and discretization as above .

Inregards with k and e values i would recommend such stratagy to solve this issue.

Try to converge a solution with low turbulent intensity and then increase the disturbances slowely by mapping the old solutions . I guess OpenFoam has that possibility.

I recommend you to make a structured mesh if the geometry is simple in Future. Also in stall regions solutions definitely oscillate , You should adopt a time averaged drag and lift Coeffcient for such application in Transient conditions. Check the resdiuals in FLUENT are they oscillting much for stalled wings.check the max and min of the coeffcients with respect to residual oscillations.

If you dont have any experimental values then i would recommend u to make mesh indipendant study in FLUENT, To make sure we are comparing the right numbers in OPENFOAM.


I have predicted the seperation point accurately for cylinders in OPENFOAM using Launder sharma turbulence model. I havent checked the other models yet.

For attached boundary layers , i think spallart allmaras Model has proven some good results in OPENFOAM. Its been reported by some Foamers in discussion Forum.

May be it helps you.. Try it..

Cheers

Dear Hrvoje, Dear Maruthamuthu
 

Dear Hrvoje, Dear Maruthamuthu,

thanks for your advices and suggestions, but unfortunately I haven't succeed in let the simulation converge... Here my today's results:

1)As reported at the beginning of this thread, my checkMesh says that:
Mesh non-orthogonality Max: 65.4365 average: 20.2284
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.899635 OK.
Moreover fvSolution says that nOrthogonalCorrectors 2. I guess it is not too bad... Am I wrong? I increased this value up to 10, but this did not improve my convergence, as expected.

2)After some tuning, I set div(phi, U) limitedLinearV 1. Should I change div(phi, epsilon) and div(phi, k) as well?

3)I applied faceLimited leastSquares 0.5 to grad schemes and Gauss harmonic limited 0.5 to laplacian schemes, as suggested by Hrvoje.

4)Yes, I have surf type wall in my constant/polyMesh/boundary file.

However, 2) and 3) did not help me to get decent results, on the contrary, the simulation became more sensitive to k and epsilon and as a consequence I obtained huge cl and cd coefficients. Thus:

5)I started with a laminar flow for 50 iterations, and then introduced some turbulence, using a small relaxation factor and increasing it step by step. In 15 "turbulent" iterations the simulation blew off.

5)I tried Launder sharma turbulence model as well, but no sign of detachment even at 24° AoA, as you can see here

What I have forgotten to say up to now is that Fluent results are close to experimental results, that's why I am a bit puzzled by OF results... Moreover, I really cannot understand what epsilon value use for my inlet and my internalField, even if I know the converged Fluent value. Is there any trick for them a part what I have already used?

Hope that some other suggestions will help me to get through these problems!

Regards,
Maddalena

Dear Hrvoje, Dear Maruthamuthu
 

Dear Hrvoje, Dear Maruthamuthu,

thanks for your advices and suggestions, but unfortunately I haven't succeed in let the simulation converge... Here my today's results:

1)As reported at the beginning of this thread, my checkMesh says that:
Mesh non-orthogonality Max: 65.4365 average: 20.2284
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.899635 OK.
Moreover fvSolution says that nOrthogonalCorrectors 2. I guess it is not too bad... Am I wrong? I increased this value up to 10, but this did not improve my convergence, as expected.

2)After some tuning, I set div(phi, U) limitedLinearV 1. Should I change div(phi, epsilon) and div(phi, k) as well?

3)I applied faceLimited leastSquares 0.5 to grad schemes and Gauss harmonic limited 0.5 to laplacian schemes, as suggested by Hrvoje.

4)Yes, I have surf type wall in my constant/polyMesh/boundary file.

However, 2) and 3) did not help me to get decent results, on the contrary, the simulation became more sensitive to k and epsilon and as a consequence I obtained huge cl and cd coefficients. Thus:

5)I started with a laminar flow for 50 iterations, and then introduced some turbulence, using a small relaxation factor and increasing it step by step. In 15 "turbulent" iterations the simulation blew off.

5)I tried Launder sharma turbulence model as well, but no sign of detachment even at 24° AoA, as you can see here
http://www.cfd-online.com/OpenFOAM_D...es/1/10994.jpg

What I have forgotten to say up to now is that Fluent results are close to experimental results, that's why I am a bit puzzled by OF results... Moreover, I really cannot understand what epsilon value use for my inlet and my internalField, even if I know the converged Fluent value. Is there any trick for them a part what I have already used?

Hope that some other suggestions will help me to get through these problems!

Regards,
Maddalena

Hello Maddalena,
 

Hello Maddalena,
Iam not a Turbulent expert to shed more light upon this problem. But i can give some tips , May be u know about it.
For external flows viscosity ratio Mut/Mu for free stream inlet should be set between 1 to 10. I used this settings in FLUENT and coupled with TI % has given good results.

In OpenFoam your epsilon values can be set correspoonding to Mut/ Mu Value. The realtionship is available in USER GUIDE FLUENT as well.

In regards with Numerics, some other FOAMERS can guide you for such unstructured grids.

Good Luck.

Hello Maddalena,
 

Hello Maddalena,
Iam not a Turbulent expert to shed more light upon this problem. But i can give some tips , May be u know about it.
For external flows viscosity ratio Mut/Mu for free stream inlet should be set between 1 to 10. I used this settings in FLUENT and coupled with TI % has given good results.

In OpenFoam your epsilon values can be set correspoonding to Mut/ Mu Value. The realtionship is available in USER GUIDE FLUENT as well.

In regards with Numerics, some other FOAMERS can guide you for such unstructured grids.

Good Luck.

Dear all, Some fresh news a
 

Dear all,

Some fresh news about Fluent-OF comparison in wing aerodynamics...

So far, I have applied realizableKE, kepsilon or Launder Sharma ke turbulence model to simulate flow around a 3D wing at Re = 250000. I specified k and epsilon boundaries value in Fluent, and applied the same values in OF as well. However, these values were too low for OF, and no detachment appeared even with a high AoA. Using k and epsilon deriving from viscosity ratio and turbolent intensity, I could finally get separation near the trailing edge. However, simulation blew off within 50 iterations and no acceptable solution could be extracted. I tried a lot of different combinations of epsilon and k values, without success.

Thus I changed the turbolence model to Spalart-Allarmas, since I wanted to be sure that the problem was somewhere in my settings and not strictly connected with the realizableKE model. I succeed to have a nice separation for AoA=24°, but the simulation crashed as usual after 100 iterations or so. I am puzzled since the simulation ran fine for the first 90 time steps, after which nuTilda increased suddently and in 10 iterations the simulation crashed. The same happened with AoA = 8°, when no separation occur.

Now, I have some hypoteses on what could be the problem:

1) is my tetra mesh not suitable for wing analysis made in OF? Maybe it is not fine enough near the wall, or it is not orthogonal enough for the solver... (see the first post of this thread for checkMesh output)

2) I noticed that I used fluentMeshToFoam to convert my Fluent file to OF, even I have a 3D mesh. I should use fluent3dMeshToFoam instead. Could it be the main cause of all my problem? I do not know, maybe a bad conversion or some odd values... However, checkMesh gives no error...

3) Do I need a fine tuning in fvSolutions and fvSchemes. If so, where to start?

Thanks in advance to everyone that give me some more hints... If you like, I can pick up my case and send it to you for a closer inspection...

Have a nice weekend!

Maddalena.

Well.... 1.) Maybe OF has o
 

Well....

1.) Maybe OF has other mesh requirements than Fluent but looking at your checkmesh results I think it should work. Is it possible to post your complete case for others to test?

2.) This should not be a problem if your mesh is transformed correct which is the case.

3.) Yes I think this is where we should start. Could you additionally post all of your fluent solver settings? I can take a short look at it on sunday.

Regards BastiL

http://www.cfd-online.com/Open
 

http://www.cfd-online.com/OpenFOAM_D...es/1/11039.jpg

Mmm.. Sorry... http://www.c
 

Mmm.. Sorry...
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif FluentSettings.jpg.tar.gz

http://www.cfd-online.com/Ope
 

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif FluentSettings.rar

Yes, this E-Mail Adress is fin
 

Yes, this E-Mail Adress is fine.

About Wall-roughtness: Did you also modify this in your FLUENT runs?

Regards

Yes, I modified OF because I'd
 

Yes, I modified OF because I'd like to be coherent with Fluent settings. In some minutes you'll get the case. Thanks.

Maddalena

Maddalena, I have taken a l
 

Maddalena,

I have taken a look at the case. Some questions and comments:

- Your mesh quality looks fine but it has no prism layers at all which is extremly poor for force prediction.. From a pure quality point of view it should run without any non-othogonal correctors. I will try.
- I do not understand your boundary conditions. I can not find an inlet as mentioned above... What patch is missing?
- I will try GAMG for pressure. This should help. Also some settings should get closer to Fluent once. I will get back to you.

Regards

Hi, I have a similar Proble
 

Hi,

I have a similar Problem with my Drag of a sphere I would love to take a look at your case - maybe I can even find some help for myself.
You can send the case to:

openfoam.messageboard at gmail.com

And I will give it a shot on a spare client.

thank you
- harly

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.