No shock in airfoil 0012 case despite of Mach number exceeds 1
5 Attachment(s)
Hi Foamers,
I'm pretty new to OpenFoam and CFD in general. I managed to get good results for low subsonic speeds on the NACA 0012. Now I'm trying to go transsonic for my thesis. I'm struggling to get a shock visible on an NACA 0012 at freestream mach number of 0.82. First I decided to use rhoSimpleFoam. Correct me if I'm wrong but there are no nonreflecting boundary conditions for this solver. So I went on and tried the following:
I would very much appreciate some critics or advise how I could go on, as I'm running out of Ideas. Thanks a lot 
Use rhoCentralFoam. That is good for shock capturing and compressible flows.

I agree with praveen. With Ma > 1 you should not use a pressurebased solver.

Thanks a lot for the hint rhoCentralFoam really works much better than the others for my case. Even if I don't understand why, as I also tried
 rhoPimpleFoam (which should be density based right ?)  sonicFoam  rhoSimpleFoam I didn't used rhoCentralFoam in the first place as the manual suggests that it does not consider turbulence. But it does. I'll put my results in here if they're finished. Thanks lot !! 
Quote:
Regards V. 
Quote:
yes, they can manage "highMach" number flows. The literature on "allspeeds" pressure based solvers is very long, and they all basically rely on similar algorithms. In practice, compressible methods allow better numerical schemes to be implemented, which reflect the physics of the problem, and naturally deal with some of the numerical difficulties presented by this kind of flow taking advantage of the mathematical nature of the equations. P.S. I am not an expert either, but recent experience showed that using a pressure based code to solver highspeed compressible flows is a waste of time. Way too many convergence and stability problems compared to a densitybased one. Best, 
Quote:
Quote:
Best, 
Quote:
Best V. 
Hi schwermetall,
It would be great if you could share your case setup as well. It would serve as a great starting point for my airfoil investigation. Thx! 
5 Attachment(s)
Hi Foamers,
first of all thanks for the support. Unfortunately I don't get a steady state solution. At first a I got two shocks on the upper and lower side in the region where they belong. But with increasing time my solution gets unsteady. There is a region of low pressure that emerges from the trailing edge disturbing the complete flow field around the airfoil. This behaviour could be seen in sonicFoam as well, see first post. What would you consider a reasonable physical time after the flow around the airfoil should reach a steady state if the conditions are as follows  freestream velocity: 277 m/s  airfoil length 1 m  domain length 40 m  Co<0.5  125 000 cells I added some picture with different time steps. I don't get a steady state after after 0.14 seconds. Very strange is, that there are two shocks on the upper side at time 0.11. After some time they occur on the lower side. thanks a lot 
Maybe it needs more iterations to reach steady state. Note that rhoCentralFoam uses global time stepping, so reaching steady state can be very slow. And moreover it uses forward euler time stepping. Atleast, some 2/3/4 stage RK scheme with local time stepping would be more robust and better for steady state problems. But this needs to be coded and is not available as a scheme. But your problem could be something else also, I cannot say.

5 Attachment(s)
It seems I found the problem concerning the unsteady behavior. I changed the mesh at the trailing edge, so that cells around the last point of the airfoil get less skewed. Below you can see pictures from physical time equals 0.152
Nevertheless the fluctuations in density and velocity at the leading edge remain. Does anyone have an idea what they could come from? I already changed the default divScheme from linear to upwind, but that doesn't help. Below my fvSchemes for the rhoCentralFoam solver: fluxScheme Kurganov;Grateful for any hints 
Quote:
Best V. 
1 Attachment(s)
hi vkrastev
I'm using RAS model with kOmega turbulence model plus wallfunction, not with resolved boundary layer. My y+ ranges between 26 and 167 (see below) . So consequently the mesh should be even a little coarser near the surface right ? Boundary consitions are fixedValue for Velocity at the inlet zeroGrad for Velocity at the outlet and fixedValue for pressure at the outlet zeroGrad for pressure at the inlet 
Quote:
supersonicFreeStream for velocity at the inlet zeroGradient for pressure at the inlet inletOutlet for velocity at the outlet waveTransmissive for pressure at the outlet Otherwise, if the incoming flow is subsonic,you can change the inlet conditions in: fixedValue for velocity waveTransmissive for pressure Regards V. PS  Now I recall that your inlet condition was subsonic, so you can try directly the second option 
Hi
thanks for the advice. I thought about changing the boundary condition, but the thing that kept from doing it was, that I couldn't find any pressure waves being reflected at the boundaries. Shouldn't I see at least anything coming back into the domain ? Nevertheless I'm going to try it and I'll report the results. By the way what do you recommend for this lInf value when using waveTransmissive? I already played with it but I'm not sure. From what I understand it is the distance behind the boundary where the given boundary value will be reached ? Regards 
Quote:
Best V. 
Quote:
I would like start with your mesh first. make the y+ to 2. Then you should use boundary conditions as suggestd by Vkrastev. Infact simply Inlet BC works good so that you can state all pressure, temperture and velocity etc... at inlet and at oulet you can make use of zerogradient B.C for all. Use sonicFoam solver this is a turbulent compressible flow. If you are using 1.6 version there are some issues with sonicFoam solver (you cannot resolve thermal boundary layer). Density based solvers are generally used for not only capturing shocks but also their interactions and these are very sensitive. where pressure based solvers are not better for these cases. use small time step for analysis. Thanks Kiran Ambilpur 
Quote:
Quote:
Quote:
Quote:
Regards V. 
I already tried sonicFoam (2.0) using different boundary conditions schemes etc etc ....
But I wasn't able to get a shock visible, with that solver. I'm using adjustTimeStep yes; with maxCo of 0.5; So thanks for the ideas, but I already tried that. 
All times are GMT 4. The time now is 05:31. 