### 12.3.3. Time Discretization

#### 12.3.3.1. Time Integration

Time integration should be carried out with the second order backward Euler scheme. This has proven to have sufficient accuracy for a wide range of applications. For turbulence (and other positive) variables, use the Bounded Second Order Implicit Euler scheme (this must be selected in ANSYS Fluent and is the default in ANSYS CFX).

The time steps should be selected to achieve a Courant number of in the LES part of the domain. For complex geometries and grids with high stretching factors, the definition of the CFL number is not always very reliable (for example, if the flow passes through a region of highly stretched cells). In such situations, estimates can be built upon the physical dimensions of the shear layer to be resolved. If cubic cells are required for resolving a shear layer (say across a mixing layer of thickness ) and a certain CFL number is to be achieved, then a time step of

| (12–33)

is required. Considering that is proportional to the RANS turbulent length scale (with a constant of order 1), this estimate may be further simplified to:

| (12–34)

where . This simplification means that the time step can be estimated on a pre-cursor RANS simulation.

You can also apply a more global estimate by assessing the through flow time, which is the time required by a fluid element to pass through the LES domain of length with velocity : . With an estimate of how many cells, , will be passed along this trajectory, one obtains .

#### 12.3.3.2. Time Advancement and Under-Relaxation (ANSYS Fluent)

There are several different settings for time advancement in ANSYS Fluent. The first choice is between the Iterative (ITA) and the Non-Iterative Time Advancement (NITA). NITA should be checked for any new application as it can result in significant CPU savings. As a general guideline, NITA works well on high quality grids and for flows with limited additional physical coupling between the equations. Within NITA, the fractional step scheme is recommended; however, one must be very cautious and conservative with the assessment of the time step size. An attempt to perform a simulation with CFL>1 can lead to an incorrect solution. In addition, one should reduce residual tolerance for all equations to 0.0001.

For the ITA schemes (everything except NITA), the segregated solvers are typically faster than the coupled solver. The optimal choice is in most cases the SIMPLEC scheme. The default under-relaxation parameters for this scheme are set for steady-state simulations. For SRS model simulations, they should be changed to values as close as possible to 1 to improve iterative convergence. Typically, the number of inner iteration loops required with SIMPLEC depends on the complexity of the flow problem. The most critical quantity is the mass conservation. Mass residuals should decrease by at least one order of magnitude every time step. With high under-relaxation and good grid quality, good solutions can often be achieved even with only two inner loops.

The coupled solver is slower per iteration, but it can lead to more robust convergence, and for complex cases can be advantageous. For the coupled solver, one would typically also specify under-relaxation values of (or close to) 1. The number of inner loops is typically 2-5. In ANSYS CFX, the coupled solver is used in all simulations.

For flows with additional physics (multiphase, combustion, and so on), the number of inner iterations per time step can increase for all solvers.

It is important to emphasize that the optimal under-relaxation factors and the optimal number of inner iterations is case-dependent. Some optimization might be required for achieving the most efficient results.

Release 18.2 - © ANSYS, Inc. All rights reserved.