I want to use Large Eddy Simulation (LES) of the Fluent code: http://cfd.me.umist.ac.uk/ercofold/d...77/test77.html

I require for your assistance concerning the launching of this technique because it's the first time that I use it, especially this two information: 1. Time step Size 2. Number of time step

Hi ck3,

i can't actually be very specific on your case and neither on LES because i'm a beginner in the field.

However, i'm doing some LES computations in turbulent channel flow (plane walls) with Fluent and maybe i can give you some guidance.

First of all, some Fluent settings. From my experience i found that a viable choice is this:

NITA - Fractional Step Method

Second Order time advancement

Unbounded Central Differencing Scheme

Dynamic Smagorinsky or Dynamic TKE (even if there is no such a big difference when no model is used)

PRESTO!

Cell-based or Least-Squares based gradient computation.

Some attention has to be paid to the time step choice. Even if the time advancement is fully implicit, the Courant number is still an issue. In fact, i performed some tests and i found that:

1) Error curves do not behaves as expected (even if with only minor differences) when time step is decreased at costant courant number equal to 1 or higher.

2) Velocity spectra in turbulent channel flow at Retau = 180 show an energy pile-up at higher frequencies when the maximum local courant number is 1 and the Unbounded Central Scheme is used for the convective term. The computations remained stable but an early instability was expected

Even if the choice of the Bounded Central Scheme is a cure for this behaviour and makes the computation stable, this should be avoided because makes the spectral resolution poorer than the already poor resolution due to the second-order/finite-volume with no explicit filtering approach employed by Fluent. I founded that with the Bounded Scheme almost all the space scales were badly affected by this choice making the LES choice more questionable than ever.

Actually, the selection of the time step and of the discretization of the convective term have shown to be the most influencing parameters in all the simulations.

So, the cure that i found reliable was obviously a time step reduction. For my channel flow case, it is based on this relation:

dt = dt+ * H^2 / ( nu * Retau^2 )

where H is the channel half-height, nu = mu / rho is the viscosity/density ratio, Retau is the turbulent reynolds number and dt+ is a dimensionless time step to specify; i found that it is nearly connected to the maximum courant number in the flow so i choosed to set dt+ = 0.3

In the turbulent plane channel, when a proper scaling is adopted, the Retau is simply 1/nu so it was simple for me to set the time step; the same is true for the grid spacing. In fact, my final selection was based on:

dt = dt+ * nu

dx = dx+ * nu

dz = dz+ * nu

rho = 1

H = 1

mu = 1 / Retau (based on the desired Retau)

dp/dx = -1 (Streamwise pressure gradient with periodic boundary condition)

I don't know if these can be proper choices in your case also, most of all because the Retau has some variation on the wavy wall. You could start using some expected values and, following the results obtained, make the proper choice; this is obviously a very time (and computational resources) consuming approach. Probably some guidilines exists for this case. You should search for them.

For grid spacing in wall parallel directions the following parameters have been used:

dx+ = 35

dz+ = 12

usually relaxed up to (but not suggested)

dx+ = 100

dz+ = 50

if the computational power is an issue.

In the wall normal direction you have no choice, a very fine grid is required near the wall, actually a DNS one, with dy+ less than one. A more relaxed spacing can be used in the center of the channel, probably up to dy+ = 20 - 30.

I don't know if in your case the proper initialization of the flow field is an issue; it was in my case so i had to add some perturbations to the initial field (a fully developed laminar flow). Because of the wavy wall this is probably not your case.

Finally, the question about the number of time steps. I suppose that, as in my case, you need to reach a stationary state and then collect statistics for some time. To see if a statistically stationary state is reached, you need to monitor the time evolution of some global parameters as the volume averaged kinetic energy or similar ones. When a steady state is reached you start to collect statistics for a certain time that, for turbulent channel flows, is usually at least 10 * H / Ut with Ut the turbulent velocity scale. A minimum of 20 collections can be assumed but much more could be required as will be clear from the averaged fiels obtained.

I hope i've been clear. If you have more questions don't hesitate to ask. Best regards

Dear Paolo Lampitella: Thank you very much for your answer. Please send me an e-mail, because I have more detail to give to you.