Onera M6 Validation with openFOAM
 

Hi,

I am trying to validate onera m6 wing (transonic airfoil) with openFoam. By the help of Micheal Aletto case (https://wiki.openfoam.com/OneraM6_by_Michael_Alletto) I run very well for the rhoSimpleFoam solver. But I want to see results of the rhoPimpleFoam to make comparison.
I can get good results for the rhoSimpleFoam, I can see the shock waves. On the other hand rhoPimpleFoam is also run but results are not good.With changing only fvSolution fvSchemes folders (from rhoPimpleFoam tutorials) for rhoPimpleFoam and using smallar deltaT I run the simulation. It is converge but results are not what I want.
So as a result, to get good result with rhoPimpleFoam what I should check , what is the reason of bad results for rhoPimpleFoam ?
Thanks for help.

some other tool that can be used? https://hisa.gitlab.io/archive.html

I didn't understand exactly that other tools mean. But I should do this with openFoam. Because it is my graduating project topic

hisaFoam is a module based on OpenFOAM (i.e. you need OpenFOAM to utilise hisaFoam). It is highly capable for compressible external flow applications. Otherwise, with the default OpenFOAM solvers, you might find yourself banging your head against the wall when something goes wrong in your high-speed compressible flow simulations.

At least, you can find that their tutorial suite contains the ONERA case as well.

(this is not an investment advice).

Hope this helps.

Did you try local time stepping

Thanks for your helps but I should also specied that I should make this analysis rhoPimpleFoam and rhoCentralFoam also. At the and we will compare the all results of pimple,central and simple. This is my final project.

You mean that I can not get good results by using rhopimplefoam ? Because I want to know whether I can solve this case by rhopimplefoam or not. rhoSimpleFoam can solve but why rhoPimpleFoam results are so far away the experimental results.

Yes I have used adjustible time step it is rearranging automatically.

You can get good results with rhoPimpleFoam. Having said that it might not be starightforward to get them. Apart from my personal experience, I don't have any evidence, I am afraid. Just be extra careful with rho* solvers, because they were developed for HVAC in mind, not for high-speed aero.

Hope this helps.

There is a tutorial where the 2d flow of a transonic airfoil is calculated with rhoPimplefoam

https://wiki.openfoam.com/NACA0012_by_Michael_Alletto

Maybe you find some hints there

There is another tutorial which simulates the supersonic flow around a sphere with rhoPimplefoam. The bow shock and expansion waves are captured desently. A suggestion how to implement a sensor to capture the high gradients around the shock is also included. https://wiki.openfoam.com/AMR_supers...ichael_Alletto

thank you so much for your helps and interest. I will look and try.

Could you please consider to share your results and the test cases herein to help others after you will accomplish your studies? I'm curious how these rho* solvers would act on this sort of engineering problems. Thanks.

Of course. If I can reach the experimental results, I will share all things :)

I couldn't exactly get the correct results but I have proceed a little. In my fvSchemes , I have written div(phid,p) $Gauss limitedLinear 1 instead of $turbulance. ( I don't know how they works or effect the results theoritically but I have write it from examples tutorials.) Then my results are more closer to experimental results in 14. second . At this point I have said it is okey it will done. :) But in 15.8 second it goes nonsense. I want to share it maybe from this point you have idea and help. If you don't , no problem I am still trying to get solution.

Could you quantify what you mean by 'nonsense'?

Log files with the minMax function object for p, T and U could be helpful.

In the worst case scenario, the Batman can be summoned. The bat signal is the limitTemperature and limitVelocity fvOptions.

Hope this helps.

Hello. I tried to simulate the onera M6 wing case with the same setting using rhoPimpleFoam as with the tutorial where I used rhoSimpleFoam. I used a local time stepping to accelerate the convergence to steady state. However after 4000 iteration steps no converged solution could be reached (I monitored the lift force which was not converged).



I found this result interesting since in principle if we underrelax rhoSimpleFoam a very similar system of equation is solved as with local time stepping and rhoPimpleFoam.


Find attached the system folder I used. I think it is enough to replace this system folder with the one of the tutorial to reproduce the results

What I can further suggest is to increase along wing resolution in the vicinity of the shock in order to capture the sharp gradients better

These are the problems i face everyday unfortunately ...
Please share your fvSchemes and fvSolution files. Then i can advice you some schemes for try. 0.orig of tutorial was well treated, i checked it. If you made some changes, let us know.
As advices:
1-Initialize with potentialFoam or just use the result of converged case with rhoSimpleFoam
2- Divergence schemes should be run to start with first orders then pass to second order(not necessarily).
3-Do not limit Pressure gradient
4- Treat div(phi,U) as directional like Gauss linearUpwindV grad(U)
5- If nonorthoganility is higher, you might treat advance in interpolation of U.

"Openfoam is just like women, treat as naive;"

@Onur Koç, and treat this answer as a sexist bullshit.