OpenFOAM, Courant number and implicit methods
I am carrying out some simulations of vortex shedding and vortex induced vibration for the case of a 3D circular cylinder at Re=10000 using Smagorinsky LES and the pimpleDyMFoam solver.
I have noticed that, although I am using the 2nd order backward implicit method for the temporal discretization, I must use adaptative time stepping with Courant number below 1.0 to get successful simulations. I would expect this behaviour with explicit methods. If Co is greater than 1.0, simulations stop due to large errors. The problem is not related to the convective discretization , because it happens even if I use limited methods like SuperBee. Even for laminar 2D simulations with Re=200 and the implicit 1st order Euler method I was unable to use large timesteps. Could someone explain why implicit methods do not allow larger timesteps when running transient vortex induced vibration simulations with OpenFOAM? Thanks, Fabio 
Because the solver is segregated. Please see the thread entitled "Courant number and implicit treatment".

If you are interested about Implicit methods and coupled solvers you can take a look here
http://openfoamwiki.net/index.php/File:Coupled.pdf.tar Regards Luca 
Stability is one thing, but accuracy another. If you want an accurate LES, you do not only need spatial resolution but also temporal. Therefore, a maxCo of about 0.2 to 0.3 is usually recommended.
Regards, Kalle 
Hi all, correct me if I'm wrong: the Backward and Euler timedifferencing schemes are simply two different approximations (the former being more accurate) of the first order time derivatives. The implicit or explicit time integration of the discretized equations is a different matter, and in OF is treated by using the fvm (fully implicit) or fvc (fully explicit) syntax inside the code. Combining the two alternatives, one can obtain some blended implicit treatment, such as for instance the CrankNicolson one. So, If all these statements are true, I guess that instabilities in timedependent problems can arise (for Co > 1) if there are some explicitly treated terms inside the discretized governing equations.
Regards V. 
Quote:
I'm very interested in the coupled solvers. I read your presentation and it looks very promising. Are you now using the new coupledMatrix solver in 1.6dev? Are you willing/able to share your coupled solvers or do you need a beta tester? Thx, Chris 
Thank you Chris,
for your comments. At the moment the developing is going very slowly cause of other priorities anyway if you are interested in more details send me an email and we can discuss about it Regards Luca 
Quote:
in the computational domain, if there is a small geonetry like a very small inlet, the maxCo will be greatly increase there. If I would like to limite maxCo to a small very, I need to reduce the time step to a small value. This directly lead to an expensive simulation. Is there any method to avoid this ? Thanks. H 
Hi Hz283,
This is a common problem in LES. You can see it as if you are trying to solve two problems with different scales in the same simulations, commonly known as a stiff problem. One way to get around such problems is to solve the two problems separately, which in this case could be to solve the inlet region in one simulation, and create an inflow library, which provides inflow to the larger domain (the inflow is then continuously repeated). Of course, such a solution may be inappropriate for your specific case. I am not aware of any general solution to your problem. K 
All times are GMT 4. The time now is 07:41. 