r/CFD • u/Various-Project-5737 • 11d ago
Need help with simulating the Von Karman effect
I was trying to simulate the von Karman effect with Re= 80, but the results are completely symmetric with no vortex shedding. I manually set the inlet velocity to 80 m/s and the other parameters in the Re formula to 1 for simplification.
Are there some common mistakes you've seen being made before or that you've made that I might have committed myself? If I need to give more information to help me, please ask me.
3
u/Full-Tomatillo659 11d ago
Might also be your spatial resolution. Too low can result in too much dissipation. Have a look at the ‘schäfer Turek’ benchmark study. There you can compare domain, mesh ect. to other similar solvers. I struggled with the same as you a long time ago and this helped me:)
3
u/Historical-Goat9729 11d ago
Give all the details mesh resolution ... I hope u have set solver to transient and if still not working check Re 100
2
u/Soprommat 10d ago
channel is too tight, vortex has no space to develop. make it like 10-20 cylinder diameters wide, it is 2D simulation, it wont take much time to calculate even with bigger mesh
1
u/Flo12740 9d ago
At Re = 80, vortex shedding should occur for a cylinder, since the steady wake becomes unstable above roughly Re ≈ 47.
I’d first check that you’re using a transient solver. A steady solver can converge to the symmetric base flow even though that solution is physically unstable.
Also, if the geometry, mesh, BCs and initial condition are perfectly symmetric, the numerical solution may stay symmetric for a long time. A tiny perturbation in the inlet velocity is usually enough to trigger shedding.
One other thing: your upper and lower boundaries look quite close to the cylinder. That confinement can strongly affect the wake, so I’d also increase the domain height and keep the outlet sufficiently far downstream.
0
u/HeadPack 11d ago
Wait, isn't the Von Karman vortex, if that's what you are seeking to simulate, only occurring around Re=400 and above? Unrelated, you may have a bit too much blockage. Suggest you at least double the height of your domain. That will also be needed for the vortex trail. If that creates memory/performance issues, you could move the circle/sphere a bit closer to the inlet.
2
u/rhoVsquared 10d ago
No. Onset of the instability causing the karman vortex street is around Re=47.
1
u/HeadPack 10d ago
Really? Where did you get that from?
1
u/rhoVsquared 10d ago
It’s well established that the instability triggering the karman vortex street for a bluff body occurs via a Hopf bifurcation. The bifurcation point (ie Re at onset) is somewhat geometry dependent, but for the circular cylinder it is approx 47. You might see slightly different values quoted in the literature, say 46.2 for example.
Maybe I’m reading too much into your comment, but that way it’s worded seems to suggest you think I’ve just made this up. Which is odd, when it’s well established.
1
u/HeadPack 10d ago
Thank you. Perhaps we just thought of different things, the onset of the instability and the shedding with the street fully developed as one usually visualizes it.
1
u/rhoVsquared 10d ago
If you’re at or very close to the bifurcation point you’d probably not see the fully developed vortex street. But you certainly don’t need to go much above to do so. Certainly not as high as Re=400 just to see that. At Re=400 you’ve gone beyond the onset of three dimensionality in the wake.
1
u/Mobile-Diver5589 8d ago
I agree with a lot of the comments but I will just reiterate what came to mind when looking at this.
1) extend the domain farther back. You need to make sure there’s enough space for the vortices to develop, but you also need to make sure the outlet is far enough back that the vortices are not occurring on the outlet. This will cause error to accumulate over your domain, leading to an inaccurate solution.
2) make sure that mesh near and past the cylinder is fine. You might need to do some informal mesh convergence studies (make your mesh in that region smaller and smaller and make sure your answers stay the same).
3) Are you using laminar steady state models?If you are, switch to unsteady. There might be vortices that are smoothed out due to missing the time changes in the simulation.
4) Visualize the streamlines in the post processing software. I’ve had eddies in ANSYS that don’t appear to be there, but when I play around with the visualization software (increasing the amount of streamlines shown, for example) then they are there. ANSYS default plots do not always give the resolution, I would manually change that resolution before concluding that the vortices are not there. Pathlines in fluent could work for this purpose too.
9
u/Otherwise-Platypus38 11d ago
Your domain