[PeterShi]

Hello all,

I am working on the project about high-lift devices(HLD,i.e. flap, slat and so on), and I try to use OpenFOAM to calculate CLmax of a certain HLD configuration.(Flow condition: Ma=0.2 Re=9e9)

However, the results show my computation tends to overestimate the lift coefficient and delay the stall angle.

Since CLmax is an important parameter of HLDs, I would like to find a way which can accurately and automatically, if possible, calculate CLmax of each case. After searching this forum, I did not find any threads related to my situation.

What I mean by "automatically" is that do we have any ways to get CLmax directly rather than calculate CL of various AOA and then get CLmax? The later one is very time-consuming.

What I mean by "accurately" is that I want to obtain similar CLmax or CL(rather than overestimate or underestimate) and the stall angle compared with experimental results.

I know this question is very complex, which is related to many factors, but any tips and suggestions are appreciated.

Regards,
Peter Shi

[jeytsav]

Dear Peter Shi

I am also investigating a High lift system case this period.

As far as I know, there is no way to just get the Clmax out of a simulation. You need to simulate over the whole range of angles of attack to do so.

Accuracy depends on way to many parameters.. Mesh type, mesh quality, mesh density, boundary conditions, wall functions, turbulence model etc.. There is no standard way to accurately capture a specific case.

What I've noticed from my study is that Fluent captures way much better the real situation with minimum "struggle" from the user's side.

With OpenFOAM, I have not yet managed to accurately capture reality.


Kind regards

[PeterShi]

Hello sir,

First of all, it is nice to meet guys from Delft! Throughout my HLD project, papers from Delft University of Technology are always good references for me. As far as I know, trailing edge high-lift devices design framework has been developed in Delft owning to excellent work done by previous MS and Ph.D. students. Moreover, this framework combines mechanical and aerodynamic modules tightly, and can evaluate aerodynamic loads, weight of high-lift systems, and so on. I am glad to tell you I am in the similar situation! I really appreciate work from Delft!

Now, let's come back to discuss our problem. My solver is OpenFOAM, which is recommended by my mentor. At this stage, I am working on 30p30n to validate my settings in OpenFOAM. The grid file was available on the website, so I transformed it into format which can be read by OpenFOAM. And numerical experiments have been carried out to find the best solution. For CL-alpha curve, results given by OpenFOAM in the linear range are quite good compared with experiments, so does the Cp distribution of AOA 16 (the literature only gives Cp distribution of that AOA). However, near the stall, OpenFOAM starts to be unreliable, it overestimates the lift coefficient, and this coefficient continues to increase even up to AOA 25! As a result, I cannot find CLmax!

As you said and literature, mesh quality plays an important role during the simulation. You know, the grid was downloaded from the website, so I cannot guarantee the quality. What I am doing is finding some rules to generate high-quality mesh for HLD.
Apart from that, I think I must figure out how to automatically get Clmax, in my opinion, calculating large range of AOAs then obtaining CLmax is an inefficient way. Processing batch might be a solution.

I am a little bit surprised that Fluent gives some reasonable results. Could you please tell me how accurate it is?(espically Clmax and stall AOA) And what are your settings in Fluent, I mean the turbulent model, algorithm, and so on?

I hope we can exchange ideas frequently. Nice to meet you again. You can reach me through my email.

Warm Regards,
Peter

[shereez234]

I will try to help you guys. Tell me more. Which turbulence model are you using? and whats your check mesh outcome?

[PeterShi]

Hello sir,

Thanks for your help.

The turbulent model I employed is K-Omega SST. According to the available literature about high-lift devices simulations, S-A has a better performance in predicting CL, while SST with transition model could better predict Cd. However, K-Omega SST model gives better performance from the global point of view.

As for the result of checkmesh operation, please see the attached file, named "The result of checkMesh". And this grid was not generated by myself, actually I got it from internet.

For your convenience, I would like to upload my folder (the uploaded compressed file 0.zip) of 30p30n with AOA=0, Ma=0.2, Re=9e9. You can look at my settings to see whether they are appropriate. Other AOAs' settings are similar, with changes of flow condition and iteration steps.

For the whole spectrum of AOAs, the attached picture named "The comparsion between experiment and OpenFOAM" compares my results with experiments found from one paper.

At this stage, I am finding ways to accurately and automatically calculate CLmax (as I mentioned in my original post). For the accuracy, I think the bad quality of grid is the culprit, now I am striving for improving the quality with every effort. For the later one, I want to use the batch processing for help, but I have not started yet. You know, calculating a lot of AoAs with intensive human interactions is so bad.

Again, thank you for your help. Any suggestions will be highly appreciated!

Best Regards,
Peter Shi

[shereez234]

Originally Posted by PeterShi

Hello sir,

Thanks for your help.

The turbulent model I employed is K-Omega SST. According to the available literature about high-lift devices simulations, S-A has a better performance in predicting CL, while SST with transition model could better predict Cd. However, K-Omega SST model gives better performance from the global point of view.

As for the result of checkmesh operation, please see the attached file, named "The result of checkMesh". And this grid was not generated by myself, actually I got it from internet.

For your convenience, I would like to upload my folder (the uploaded compressed file 0.zip) of 30p30n with AOA=0, Ma=0.2, Re=9e9. You can look at my settings to see whether they are appropriate. Other AOAs' settings are similar, with changes of flow condition and iteration steps.

For the whole spectrum of AOAs, the attached picture named "The comparsion between experiment and OpenFOAM" compares my results with experiments found from one paper.

At this stage, I am finding ways to accurately and automatically calculate CLmax (as I mentioned in my original post). For the accuracy, I think the bad quality of grid is the culprit, now I am striving for improving the quality with every effort. For the later one, I want to use the batch processing for help, but I have not started yet. You know, calculating a lot of AoAs with intensive human interactions is so bad.

Again, thank you for your help. Any suggestions will be highly appreciated!

Best Regards,
Peter Shi

Okay Hi again. I have had a look at your settings and mesh. let me point out a few things one by one.

1. Experiments and CFD simulations don't always match and they don't need to. So CL_max and Stall Angle can vary a little when compared to experiments and that is not a problem unless it is off significantly. So you don't worry too much about that okay. However, you have to try and replicate the conditions of an experiment in the simulation as much as you can ( such as inlet velocities, reference lengths, turbulence levels, etc, etc...).

2. You are mentioning that Re = 9e9 which is like 9,000,000,000. This isn't right. Flight conditions and simulations usually vary from 100,000 to 50,000,000 ( 50 million). So you have something wrong there in your details. However, I checked your folder and Uref = 68, Nu = 4.33e-06 and Lref = 0.55 creates Re = 9 million which might be correct if that's what you intended to mention here.

3. Stall is a complicated phenomenon. It is sensitive to a lot of factors ( in experiments and in CFD). I checked that your inlet kinetic energy is 0.027 and omega is 3947. For me personally these values are too high.
I would suggest that you use this formula to calculate k and omega at inlet and give another try for simulation

k_inlet = 1e-03 * (U_inlet)^2 / (Reynolds number))

omega_inlet = 5 * (U_inlet) / (Length of Domain).

3. I see that you are using a steady state simulation. This is okay for the linear part when the flow is attached. but as soon as the flow starts to separate there will be unsteady transient vortices with periodic shedding. read about strouhal number and choose a time step accurate enough to capture this. The recommended way is to use Courant number <1 and use pisoFoam for simulations. If you don't have patience and time and you wish to hurry up and go for a faster unsteady simulation then search the forum for transientSimpleFoam and you can use Courant number < 200 (typically, you can go higher but I wouldnt recommend it) and perform a Pseudo Unsteady simulation.

4. Change your gradschemes from Gauss linear to cellLimited Gauss linear for default and Gauss linear for only pressure. I mean:
default cellLimited Gauss linear 1;
grad(p) Gauss linear;

5. In your fvSolution decrease relTol for U,k, omega. I usually use 0.1 or 0.01 for p as relTol and 0.001 for U,k,omega,etc..

6. Your mesh is okay for checkMesh. However, I don't know if the mesh has Y+ < 1. This is ideal to capture correct Cl_Max and Stall angle. So I would advice you to make it by yourself.

7. In your FvSolution for relaxation parameters change U to 0.7 rather than 0.8. It's said that U_relax + p_Relax = 1 is the best settings. so 0.7(U) + 0.3(p) = 1 would be favorable.

Hope this helps.

[PeterShi]

Originally Posted by shereez234

Okay Hi again. I have had a look at your settings and mesh. let me point out a few things one by one.

1. Experiments and CFD simulations don't always match and they don't need to. So CL_max and Stall Angle can vary a little when compared to experiments and that is not a problem unless it is off significantly. So you don't worry too much about that okay. However, you have to try and replicate the conditions of an experiment in the simulation as much as you can ( such as inlet velocities, reference lengths, turbulence levels, etc, etc...).

2. You are mentioning that Re = 9e9 which is like 9,000,000,000. This isn't right. Flight conditions and simulations usually vary from 100,000 to 50,000,000 ( 50 million). So you have something wrong there in your details. However, I checked your folder and Uref = 68, Nu = 4.33e-06 and Lref = 0.55 creates Re = 9 million which might be correct if that's what you intended to mention here.

3. Stall is a complicated phenomenon. It is sensitive to a lot of factors ( in experiments and in CFD). I checked that your inlet kinetic energy is 0.027 and omega is 3947. For me personally these values are too high.
I would suggest that you use this formula to calculate k and omega at inlet and give another try for simulation

k_inlet = 1e-03 * (U_inlet)^2 / (Reynolds number))

omega_inlet = 5 * (U_inlet) / (Length of Domain).

3. I see that you are using a steady state simulation. This is okay for the linear part when the flow is attached. but as soon as the flow starts to separate there will be unsteady transient vortices with periodic shedding. read about strouhal number and choose a time step accurate enough to capture this. The recommended way is to use Courant number <1 and use pisoFoam for simulations. If you don't have patience and time and you wish to hurry up and go for a faster unsteady simulation then search the forum for transientSimpleFoam and you can use Courant number < 200 (typically, you can go higher but I wouldnt recommend it) and perform a Pseudo Unsteady simulation.

4. Change your gradschemes from Gauss linear to cellLimited Gauss linear for default and Gauss linear for only pressure. I mean:
default cellLimited Gauss linear 1;
grad(p) Gauss linear;

5. In your fvSolution decrease relTol for U,k, omega. I usually use 0.1 or 0.01 for p as relTol and 0.001 for U,k,omega,etc..

6. Your mesh is okay for checkMesh. However, I don't know if the mesh has Y+ < 1. This is ideal to capture correct Cl_Max and Stall angle. So I would advice you to make it by yourself.

7. In your FvSolution for relaxation parameters change U to 0.7 rather than 0.8. It's said that U_relax + p_Relax = 1 is the best settings. so 0.7(U) + 0.3(p) = 1 would be favorable.

Hope this helps.

Hello sir,

Your response is DEFINITELY my big help.

Yes, Re=9e9 is my typo. The number I used in the simulation is 9e6.

I will have a try according to your advice, and any progress will be posted here, if any.

I have time as well as patience, owing to your help, I have the confidence to get this job done. Thank you.

Best Regards,
Peter

[PeterShi]

Originally Posted by shereez234

Okay Hi again. I have had a look at your settings and mesh. let me point out a few things one by one.

1. Experiments and CFD simulations don't always match and they don't need to. So CL_max and Stall Angle can vary a little when compared to experiments and that is not a problem unless it is off significantly. So you don't worry too much about that okay. However, you have to try and replicate the conditions of an experiment in the simulation as much as you can ( such as inlet velocities, reference lengths, turbulence levels, etc, etc...).

2. You are mentioning that Re = 9e9 which is like 9,000,000,000. This isn't right. Flight conditions and simulations usually vary from 100,000 to 50,000,000 ( 50 million). So you have something wrong there in your details. However, I checked your folder and Uref = 68, Nu = 4.33e-06 and Lref = 0.55 creates Re = 9 million which might be correct if that's what you intended to mention here.

3. Stall is a complicated phenomenon. It is sensitive to a lot of factors ( in experiments and in CFD). I checked that your inlet kinetic energy is 0.027 and omega is 3947. For me personally these values are too high.
I would suggest that you use this formula to calculate k and omega at inlet and give another try for simulation

k_inlet = 1e-03 * (U_inlet)^2 / (Reynolds number))

omega_inlet = 5 * (U_inlet) / (Length of Domain).

3. I see that you are using a steady state simulation. This is okay for the linear part when the flow is attached. but as soon as the flow starts to separate there will be unsteady transient vortices with periodic shedding. read about strouhal number and choose a time step accurate enough to capture this. The recommended way is to use Courant number <1 and use pisoFoam for simulations. If you don't have patience and time and you wish to hurry up and go for a faster unsteady simulation then search the forum for transientSimpleFoam and you can use Courant number < 200 (typically, you can go higher but I wouldnt recommend it) and perform a Pseudo Unsteady simulation.

4. Change your gradschemes from Gauss linear to cellLimited Gauss linear for default and Gauss linear for only pressure. I mean:
default cellLimited Gauss linear 1;
grad(p) Gauss linear;

5. In your fvSolution decrease relTol for U,k, omega. I usually use 0.1 or 0.01 for p as relTol and 0.001 for U,k,omega,etc..

6. Your mesh is okay for checkMesh. However, I don't know if the mesh has Y+ < 1. This is ideal to capture correct Cl_Max and Stall angle. So I would advice you to make it by yourself.

7. In your FvSolution for relaxation parameters change U to 0.7 rather than 0.8. It's said that U_relax + p_Relax = 1 is the best settings. so 0.7(U) + 0.3(p) = 1 would be favorable.

Hope this helps.

Hi Shereez,

How is it going?

I've already searched for transientsimpleFoam, and it is your thread actually. I assume it is the solver developed by yourself, since I did not find it within OpenFOAM. On the other hand, I found pimpleFoam, it might be a good candidate if I want to use large time step, i.e. large CFL number.

My program is still running, the computation is really slow in order to insure CFL<1, but I guess tomorrow I will get the result.

Today, I am generating my own mesh. However, checkMesh always tells me that my mesh has a lot of high-aspect ratio or non-orthogonal cells. Do you have any suggestions for generating mesh of high-lift devices? My grid generator is pointwise.

Thanks. Any progress will follow.

Best Regards,
Peter

[jeytsav]

Dear Peter Shi

Sorry for my late reply.

I d like to thank you for the nice words about Delft. I am currently doing my MSc there. This period I am doing an internship trying to simulate a high lift system with openFOAM.

My main objective is to do a mesh independence study and not to focus on Clmax and stall angle. (you will notice in my simulation that I am not solving for a lot of angles of attack near stall.

I am using SA model and recently I have switched to kwSST (without any results yet)

Please allow me to post my /0 and /system folders here along with my results up to now. I have also solved with Fluent to validate my results using the exact same mesh.

Cl.png Cd.png


My mesh is around 20mil elements and has a y+~1. Due to the later, I am not using any wall functions.

Notice the great difference between the two simulations. Fluent captures almost perfectly the experimental results. I am struggling to make openFOAM more accurate but I am probably missing something with the settings.

It can't be the mesh density cause I also solved for a 76mil mesh with only slight improvement.

My current mesh type is trias on the surface and tetras in the volume.

I am now testing another mesh type - quads on surface, tetras in volume - and this leads to slightly better results, however still worse than Fluent.

Regarding your question about non-orthogonality, high aspect etc., I also have the same problem. In my case it is due to the very small first layer thickness, causing violating cells in the first layers, (due to my low y+). But something like this is unavoidable.

I will be grateful for any suggestion/advice regarding my case


Kind regards

[shereez234]

I can't tell you much about pointwise. I am a fan of ICEM CFD. But I can tell you that if you decrease Aspect Ratio in Far Field your grid quality will improve significantly.

[PeterShi]

Originally Posted by jeytsav

Dear Peter Shi

Sorry for my late reply.

I d like to thank you for the nice words about Delft. I am currently doing my MSc there. This period I am doing an internship trying to simulate a high lift system with openFOAM.

My main objective is to do a mesh independence study and not to focus on Clmax and stall angle. (you will notice in my simulation that I am not solving for a lot of angles of attack near stall.

I am using SA model and recently I have switched to kwSST (without any results yet)

Please allow me to post my /0 and /system folders here along with my results up to now. I have also solved with Fluent to validate my results using the exact same mesh.

Attachment 53878 Attachment 53879


My mesh is around 20mil elements and has a y+~1. Due to the later, I am not using any wall functions.

Notice the great difference between the two simulations. Fluent captures almost perfectly the experimental results. I am struggling to make openFOAM more accurate but I am probably missing something with the settings.

It can't be the mesh density cause I also solved for a 76mil mesh with only slight improvement.

My current mesh type is trias on the surface and tetras in the volume.

I am now testing another mesh type - quads on surface, tetras in volume - and this leads to slightly better results, however still worse than Fluent.

Regarding your question about non-orthogonality, high aspect etc., I also have the same problem. In my case it is due to the very small first layer thickness, causing violating cells in the first layers, (due to my low y+). But something like this is unavoidable.

I will be grateful for any suggestion/advice regarding my case


Kind regards

Hello John,

I am so sorry for my late reply, as a matter of fact, I just finished a technical report after literature review. Here are some guidelines to improve the accuracy:
1. Using compressible solver instead of incompressible solver. Specifically, you can try rhoSimpleFoam rather than simpleFoam;
2. Employing unsteady solver near flow separation. As you know, I am interested in Clmax, hence this point is important for me. Since when the flow separates, actually it is an unsteady problem-vortex is shed from upstream.
3. Considering the transitional turbulent models. Transition actually is quite important in the simulation of muti-element airfoil. However, most solvers do not have this capability. For OpenFOAM, there is a transitional model available, which is kklomega. However, this is not the popular one I saw in the papers, instead, SST transitional model is widely used. For how to include this model into OpenFOAM, please see following link: http://www.tfd.chalmers.se/~hani/kur...transition.pdf
4. Grid quality does play a crucial role during your simulation. You pointed out your results are mesh independent. It might be true, but I would like to say, that your result does DEPENDENT on the mesh quality, though it is INDEPENDENT on the number of the grid. Poor grid will lead to unsatisfactory or even unphysical conclusion, so improving your grid quality is necessary. Typical high quality grid in 2D case is displayed in the attached picture. As you can see, besides satisfying normal criteria (like aspect ratio and orthogonality), the grid is refined in the certain region. I guess he refined his mesh according to the flow field, maybe adaptive mesh will help, which is also available in OpenFOAM.

Regarding to your situation, I would like to give you some advice, you can have a try and see whether it will work.
1. Change the boundary type in 0/nut for inlet&outlet from fixedValue and zeroGradient respectively, to calculated;
2. Chaenge the boundary type in 0/U for outlet from fixedValue to pressureInletOutletVelocity;
3. Change your gradScheme in fvsheme from default cellLimited leastSquares 1.0 to Gauss liner;
4. Change your divSchemes from
divSchemes
{
default none;
div(phi,U) bounded Gauss linearUpwindV grad(U);
div(div(phi,U)) Gauss linear;
div(phi,nuTilda) bounded Gauss linearUpwind grad(nuTilda);
div((nuEff*dev2(T(grad(U))))) Gauss linear;
}
to
divSchemes
{
default none;
div(phi,U) bounded Gauss linearUpwindV grad(U);
div(phi,nuTilda) bounded Gauss limitedLinear 1;
div((nuEff*dev2(T(grad(U))))) Gauss linear;

}


That's all. Above suggestions are based on the papers and my personal experience, in fact, I am also investigating some of points currently. I hope these suggestions will work and both of us can improve the accuracy.

PS:At this time, I do not know why I cannot upload a picture, later, I will upload it. And you said you want to use quads on the surface, great, just have a try, a video said quads have some advantages over ter. Moreover, I have KOmega-SST results for 30p30n with the AOAs from 0 to 25 degrees, you can compare yours with me.

Best regards,
Peter

[PeterShi]

Hello guys,

How is it going? There is some progress of mine.

Instead of testing 30p30n, I turned to NHLP-2D, another high-lift configuration, since it has more data available in public.

I attached four pictures of my results:
1)CD comparison of different turbulent models with experimental results;
2)CL comparison of different turbulent models with experimental results;
3)CM;
4)Grid Dependency.

Those results look fine to me. Now, I am using compressible solver to carry out more tests.

As a suggestion, mesh quality is super important during the calculation.

And I hope you can report your progress of calculating high-lift devices.

Best regards,
Peter

[jeytsav]

Dear Peter

I am really busy right now in completing my study so please excuse me for not responding on time.

I have changed some settings to my solver and managed to get better results.

I can confirm that kOmegaSST capture better the case for higher angles and it lies a bit closer to the experimental results.
I can also confirm the inability to capture the results correctly after stall.

I will try to post some graphs along with my settings, the sooner the possible. Please excuse me but I am really in a hurry to meet deadlines.

I will get back to you soon

kind regards