11.2.4. Numerics Settings for SRS Models

For Scale-Resolving Simulations (SRS), specific discretization and solver settings are required to achieve optimal accuracy with minimal numerical effort. The recommendations given below should be considered as a starting point for your specific flow application and are not generic, but problem dependent. The recommendations are based on incompressible, single phase flow without chemical reactions or other complex additional physics. In case your simulation features additional complex physical effects, it requires adjusting the recommended solver settings accordingly. In most cases, this will mean that a higher effort must be invested into the coupling of the equations (for example lower time step, reduced under-relaxation, higher iteration count, smaller residuals), in order to avoid a de-coupling of different physical phenomena.

For SRS models, it is generally recommended to use the pressure-based solver, as it offers optimized schemes for resolving turbulence relative to the density based solver.

For Scale-Resolving Simulations, optimal numerics settings are essential for achieving accurate results in an acceptable time frame. The reason is that at the SRS models operate at the resolution limit of the provided grid where the smallest scales are of the order of the grid spacing and the time resolution. Numerics settings therefore have to be chosen to provide an optimal balance between accuracy and robustness.

It is generally recommended to initialize the solution from a (reasonably) converged RANS simulation.

11.2.4.1. Time Discretization

For Scale-Resolving Simulations, the resolution of the turbulent structures in time is essential for the success of the simulation. This is, to the largest extent, defined by the selected time step. As the SRS model is operating at the grid limit, you should select a time step that ensures a Courant-Friedrichs-Levy (CFL) number of

(11–5)

The CFL number is computed by the solver and can be checked based on an initial RANS simulation, for example. It is important to emphasize that this is not a numerical limit and that the solver will be able to sustain much larger CFL numbers. In complex applications, there will always be limited regions of fine cells or large velocities and you should not restrict the CFL number based on such zones. The recommendation of CFL =1 should be applied in the main SRS region in combination with a uniform isotropic grid. It is recommended that you vary the time step for each type of application and explore its optimal value. This can substantially save on computing costs.

The time derivative should be computed by the Second Order Implicit option. (See User Inputs for Time-Dependent Problems for guidelines on setting solution parameters for transient calculations in general.)

11.2.4.2. Spatial Discretization

For SRS models, it is important to minimize the numerical dissipation of the scheme in order to avoid damping of the smallest scales by numerical dissipation. For spatial discretization, the choice is between the Central Differencing (CD) scheme (see Central-Differencing Scheme in the Theory Guide) and the Bounded Central Differencing scheme (BCD) (see Bounded Central Differencing Scheme in the Theory Guide). The Central Differencing scheme is the least dissipative and provides the highest resolution accuracy for the smallest scales. Especially for aero-acoustics simulations, where the spectral content at higher frequencies can be important, this is a desirable feature. However, Central Differencing schemes are prone to solution oscillations (checker boarding) in the velocity field. When using the Central Differencing scheme, it is therefore important to provide a high quality mesh (no mesh jumps, isotropic cells and high resolution in critical zones) and to avoid large time steps (the CFL number should be smaller than 1 in the main SRS region). It is recommended that you visually monitor the solution regularly in order to avoid wasting computational resources. In case oscillations appear, the choice is to: improve the mesh; reduce the time step; or to switch to the slightly more dissipative, but also more robust Bounded Central Differencing scheme. In many complex applications, the Bounded Central Differencing Scheme is the numerics option of choice. It typically provides sufficiently low dissipation to allow the turbulent structures to evolve, but, at the same time, is robust enough to handle non-optimal grids as they are typically encountered in industrial simulations. In addition, the Bounded Central Differencing scheme is also suitable for hybrid methods like SAS, DES, SDES, and SBES, and will provide stable solutions in RANS regions, with highly stretched grids and with a CFL number larger than 1. For ELES, the numerical scheme in the LES zone can be selected independently from the settings in the RANS zone. The RANS region can then be computed with standard higher-order upwind schemes and the LES zone can be covered by either the Central Differencing scheme or the Bounded Central Differencing scheme.

For the gradient calculation, it is recommended that you select the Least Squares Cell Based option, or the Green-Gauss Node Based option, to ensure a second-order interpolation on non-orthogonal grids.

For pressure interpolation, it is recommended that you use the second-order scheme, or the body-force-weighted scheme. Due to its higher dissipation, the PRESTO! scheme (see Pressure Interpolation Schemes in the Theory Guide) can result in a delayed formation or damping of turbulent structures. It is therefore not recommended for SRS.

11.2.4.3. Iterative Scheme

The selection of the iterative scheme will mostly affect the computational costs as the cost per iteration between these methods is rather different. However, recommendations are not straightforward, as the higher cost per iteration of a scheme can be offset by faster convergence within the time step.

The fastest scheme is the Non-Iterative Time Advancement (NITA) scheme (see Non-Iterative Time-Advancement Scheme in the Theory Guide as well as Setting Solution Controls for the Non-Iterative Solver). This scheme typically works well for limited LES zones and high quality meshes. It is also important to ensure a low time step of a CFL number below 1. For the NITA scheme, all explicit under-relaxation factors are, by default, set equal to one. With NITA, it has slight advantages to use the fractional step method if there is no involvement of more complex physics, when otherwise the PISO scheme can be more beneficial.

In case the application is too complex for the NITA scheme to provide a solution, the iterative SIMPLEC (SIMPLE vs. SIMPLEC) or PISO (PISO) schemes are the next possible option. They should be preferred relative to the SIMPLE scheme, as they show faster convergence per time step and can be run with more aggressive under-relaxation (higher values equal to 1 or close to 1). If such settings prevent convergence within the time step, then check if your time step is small enough for maintaining CFL numbers below 1 in the SRS region – if not, then try reducing . If this is not possible, or does not lead to satisfactory convergence, then reduce the under-relaxation factors to values between the default settings and 1. For skewed meshes or meshes with problematic quality, the reduction of explicit relaxation factor for pressure correction down to 0.7 from 1 can be very helpful.

11.2.4.3.1. Convergence Control

The convergence criterion within each time step will strongly affect solution costs, as a low criterion will result in an increased number of iterations. It is not possible to provide general recommendations, as the required residual depends on the application. The most relevant residual in the SRS models is the continuity residual. It should be converged by approximately 2 orders of magnitude per time step for a CFL number ~ 1. This should be achievable with around 5-10 maximum iterations per time step for flows involving no other physical models. Be sure to check the impact of convergence on your solution to ensure that the residual is reduced to a level consistent with your problem.

For simulations with small CFL values, the Extrapolate variables option (available in the Run Calculation Task Page) can be very beneficial. This can substantially reduce the number of iterations within the time step up to 40% when the convergence control is based on the convergence criteria.

In case your simulation requires the combination of additional physical models, such as combustion or multiphase, a reduction of the under-relaxation factors might be required. In this case, the number of maximum iterations per time step can be increased to achieve the desired residual reduction.

For hybrid RANS/LES simulations, such as the SAS, DES, SDES, and SBES models, there can be situations where the RANS portion of the flow limits convergence (for example, due to poor grid quality). In such cases, the application of the coupled solver should be considered. For the coupled pressure-based solver, each iteration is typically more expensive than for the SIMPLEC algorithm, but this is at least partly offset by faster convergence. The recommendations concerning residuals are similar to the SIMPLEC method, but the maximal number of iterations can be reduced to values as low as 2-5 for highly unstable flows, and 5-10 for more sensible flows and acoustics simulations.


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