[chengdi]

Hi, everyone

I am working on naca0012 validation case in NASA TMR using the grid (the most coarse one for now) and model provided by TMR. It is required to join DPW 6.

2D case with Mach 0.15 and Re=6e6. Seems easy at first glance.
However, there are a lot of obstacles and traps!!! Including:
1. max aspect ratio of grid (most coarse one, familty-II) is 2.4E7! It did not past the checkMesh. However it can be run.
2. SA model in OpenFOAM is not a standard SA.
3. The effective Prandtl number of original sutherlandTransport model of OpenFOAM is not 0.72 but 0.69. (sutherlandTransport is using Eugene's equation rather than Prandtl number approach)
4. The turbulent Prandtl number of EddyViscosity is 1.0 by default.
5. No Riemann BC in OpenFOAM.
6. The 500*cord far field boundary is so large that I need to run too many timesteps to reach steady state with an unsteady solvers. However, there is only one compressible steady state solver available in OpenFOAM 201612+ (the rhoSimpleFoam) which seems not very good for highly compressible flow.

Now I am running into turbulence. I just found that there is no example case of compressible SA model in OpenFOAM 1612+ and foam extend 4.0.

And I found that the initial condition and solver configuration existing in incompressible SA model case does not work in compressible SA case becasue of lacking `0/alphat` field.

And the alphat field is not thermal diffsivity. It seems like `density*thermal diffusivity` because its dimension must be [1 -1 -1 0 0 0 0]. (confirmed by the implementation of SA model code)

I am totally frustrated by this validation case. Is there anyone have any experience on doing DPW-like verification with naca 0012 using OpenFOAM?

[Bernoulli666]

I run the simulation with the parameters in the folder and Mesh size 897 and seems that results are very similar to the nlrc ones.

[chengdi]

NASA TMR requires that the case should be calculated using compressible code rather than simpleFoam (an incompressible code). I tried to used rhoCentralFoam in unsteady manner, it works. However the time is too long. I also tried to use rhoSimpleFoam, it is not working.

[Bernoulli666]

You can also use compressibile solvers for uncompressible flows. If you look in the tutorial folder "incompressibile" there are cases solved with simple algorithm.


Sent from my iPad using CFD Online Forum mobile app

[chengdi]

Yes, I can solve it even with potentialFoam. However, according to NASA's comment, the solver is required to be an incompressible solver.

[Flowkersma]

Hi,

My first question is, why are you using compressible solver? I have run the same case with simpleFoam and kOmegaSST turbulence model and I got very similar results to NASA's results.

1. High aspect ratios does not seem to be a problem for OpenFOAM even though checkMesh gives an error.
2. This depends on which OF version you are using? Older releases are using the not recommended one with fv3 term. I think that OF foundation is using now the "good" implementation without fv3 term. However, I am not sure about OF+. Unfortunately, foam-extend is probably still using the fv3 term implementation.
3-4. If the compressibility effects are almost negligible, do we care?
6. This flow is not highly compressible so I would use simpleFoam or if you want to stick to compressible solver then rhoSimpleFoam.

Regards,
Mikko

[chengdi]

Hi, Mikko

For your questions:

1. Not just high aspect ratio problem. The highest AR element is located at the the wake baffle and it is very orthogonal rectangular element. The non-orthogonality might be the worst factor. The max angle is > 80 degree.

2. I am using compressible solver because the verification case requires that. And I just want to make sure the OpenFOAM 201612+ can be used to produce a result almost exactly as CFL3D/FUN3D and TAU of DLR. So I can assure that the program is correctly coded and can be used to deal with external aerodynamic problems such as DPW6.

3. For application, it is negligible and I will definitely use incompressible solver, however, this is a verification case. I must follow the guide as closely as I can.

4. rhoSimpleFoam is very difficult to run without divergence or thermophysical problem.

[Iain_symthe]

Originally Posted by Bernoulli666

I run the simulation with the parameters in the folder and Mesh size 897 and seems that results are very similar to the nlrc ones.

Thanks for attaching the zip file with your values. Can you also share your validation results (OF simulations with data) in text files. How many steps did you need to run for convergence? Looking at your 0/U and 0/nut files it looks like you are running a Re = 3M case (87/3.e-6) for Lref = 1



I am trying to run the Re = 10^6 case as outlined in

https://www.openfoam.com/documentati...irfoil-2d.html
using the n0012_897-257.p3dfmt file.


I had to do

plot3dToFoam -noBlank n0012_897-257.p3dfmt

followed by
autoPatch -overwrite 15


to generate a proper boundary file (with inlet, outlet, front, back and airfoil) in it. I have used values for U_alpha, nu and nuT as prescribed in the OF validation page and I have run the simulation with
simpleFoam for 10000 steps but it has still not converged.


It will be helpful if someone has run this case (Re = 1e6) to completion and compared their results to data as in the OF validation page.
I have attached my setup file (without polyMesh as it is too large).



Thanks
Iain