I have the following questions about LES: 1.I hear most LES uses explicit time marching scheme, Is the implicit marching very time-comsuming? Did someone try a full implicit scheme? 2.If explicit scheme is used,I read from some papers that the diffusion terms normal to the wall should to be treated implicitly to avoid numerical instability. So I wanna know if these terms must be treated implicitly in all LES? 3.When the diffsiion terms are treated implicitly, Should the eddy viscosity also be treated implicitly ? A implicitly treated eddy viscosity would bring nonlinearity to the solution.

Any comment is welcome thanks ben

LES simulations are required to be accurate in time. This tends to limit the maximum time step to something around the explicit stability limit making implicit schemes expensive and unnecessary.

There are exceptions where grid spacing is very fine for reasons other than accuracy. The most common is strong grid clusterting near solid surfaces in order to apply accurate boundary conditions. Treating the diffusion terms in an implicit manner will allow the time step to be raised to a reasonable value for the bulk flow (the near wall flow is not accurately resolved). There is no need to treat the convection terms implicitly because the velocity is small.

The above works for duct flows but not something like a backward step. The problem area here is just downstream of the corner which has a strongly clustered grid from the upstream boundary layer but significant velocities in the direction of the fine grid spacing due to large (w.r.t to the fine grid spacing) vortices. The convection terms in this direction will need to be treated implicitly.

The implementation of an implicit scheme in one direction only can be done accurately and inexpensively but it is a bit awkward to handle in a general manner. Faced with this many have adopted a general implicit treatment in all three directions and taken a significant hit in computational efficiency and, often, accurate handling of the non-linearity.

If you use a reasonable wall function treatment then there is no grid clustering near solid boundaries and one can stick with efficient explicit schemes (excluding the pressure which has to be treated implicitly at low Mach numbers).

There is no need to treat the eddy viscosity implicity because it is a very poor model for the instantaneous grid scale turbulent stresses it represents. The success of the model relies on being reasonable in a statistical sense (i.e. over a long time period and not instantaneously) and also being very small relative to the resolved (unmodelled) turbulent transport.

Dear andy ,you really helped me and I really learnt a lot from your comment. Can I sumarrize as following:

1.When using explicit schemes and the grid is very fine,the time step should also be very small,otherwise the calculation may suffer numerical instability.(implicit schemes dont have this problem)

2.When no wall function is employed,the grid near the wall should be very fine relative to the bulk flow,and either we use very small time step size or we treat some terms implicitly to make the simulation stable.

3.I guess the most efficient simulation for a general geometry turbulent flow should use wall functions and hence reduce the grid resolution and time step size and also all terms can be treated explicitly ,and thus the computational cost will be greatly reduced.

4.About the wall models :what is the most efficient and easy to program one ? Some referrance would be appreciated.

5.When programming the dynamic model ,how is the test filter averaging done? When the test filter width is twice the grid filter width ,I just used the average of the neighbouring six nodes' value to get the explicitly filtered field(uniform grid), I dont know if it is the best way to average.

6.When a full implicit scheme is used, and the time step is chosen to be big enough to reduce the total computational cost ,can we still get a reasonable statistical solution?

Correct me if I am wrong,Thanks again.

best regards

ben

Without going into a bunch of detail, here are some thoughts. Take the governing equations and write them like this:

dU/dt = F1 + F2 + F3 + ...

where U is the integration vector and F1 might be the convective term, F2 might be the diffusion term, F3 might be a reactive term, etcetera. Now, in principle, one could integrate all terms using an exceptional implicit method like Radau IIA. With an error controller, the user can select an error tolerance that allows the resolution of the desired physical processes but does not allow the time step to descend below this value. This time step is the fastest time scale you need to resolve. In reality, you're probably going to need a different strategy on how to determine it. Lets call the fastest relevant physical time scale of the problem Tp.

Next, linearize the terms

d(F1)/dU, d(F2)/dU, and d(F3)/dU ...

about some useful state for each grid point. Compute the eigenvalues of each matrix. Take the eigenvalue which has maximum magnitude. The reciprocal of this represents the fastest timescale of that term; T1, T2, and T3 etcetera. The eigenvalues are inversely proportional to the grid spacing raised to the order of the derivative. This means that second derivative terms will have huge eigenvalues when the grid clusters. To determine the stiffness of each term, compute

T1/Tp, T2/Tp, T3/Tp, ...

If any of those terms gets much less than 1/10 to 1/100, the term might best be integrated implicitly.

If the system of equations was based on the compressible equations and not the incompressible or low-Mach equations, consider a coupled, Implicit/Explicit, Runge-Kutta integrator. Here are two new ones and you should check the "cited by" also

http://scholar.google.com/scholar?hl=en&lr=&q=Calvo+runge-kutta+Frutos+Novo+Linearly+implicit+

If there is a constraint manifold to which the solution must adhere, you could use an Implicit/Explicit multistep method. The key papers here begin with: UM Ascher, SJ Ruuth, BTR Wetton

http://scholar.google.com/scholar?hl=en&lr=&q=ascher+implicit+multistep+explicit+Wetton+Ruuth&btnG=Sea rch

Also,

http://www.cfd-online.com/Forum/main.cgi?read=34955