Setting Parameters for the Segregated Approach

Here, you set the model and solver parameters for the segregated approach

To set the model parameters:
  1. Select the Continua > [physics continuum] > Segregated Flow node and set Convection to one of the following discretization schemes for the convective flux:
    • 2nd-order—this is the default and suitable for most cases. It is an upwind convection scheme of second order accuracy, which is a good compromise between robustness and accuracy.
    • 1st-order—select the first-order upwind convection scheme when a higher-order scheme fails to converge, or in order to obtain an initial solution before switching to a higher-order scheme.
    • MUSCL-3rd order/CD—this scheme is a blend between a MUSCL 3rd-order upwind scheme and the 3rd-order central-differencing reconstruction scheme. It provides improved (reduced) dissipation when compared with the second-order scheme. At the same time, it is robust and capable of simulating steady and unsteady flows from incompressible to high-speed compressible regimes.

      You can set the Upwind Blending Factor—the proportion of upwind differencing—using the Coupled Flow > Bounded Differencing node. The default value provides the most robustness for the scheme. Reducing it would, in principle, increase accuracy. However, unless you are thoroughly familiar with the theoretical aspects of bounded differencing, do not change this property. The default value reflects optimization for accuracy and performance.

    For more information, see Flow Models Reference—Properties Lookup.

To set the solver parameters:
  1. For unsteady simulations, select the Solvers > [Implicit Unsteady/PISO Unsteady] node and set the following properties:
    • Time-Step—specify the physical time-step size. The choice of time-step is an engineering judgment (in the same way as grid refinement). The convective Courant number is a helpful indication for selecting the time step size: for time-accurate simulations, the convective Courant number should be 1.0 on average in the zone of the interest. This value implies that the fluid moves by about one cell per time step. For more information, see Segregated Flow Guidelines—Transient Time-Step and Inner Iterations.
    • Temporal Discretization (for Implicit Unsteady)—sets the temporal discretization scheme. The default is 1st-order. To use high-accuracy temporal discretization, set this property to 2nd-order. High-accuracy discretization schemes give faster unsteady solutions by using larger time steps and are more accurate. However, they are harder to stabilize and require more attention to mesh quality. Start with the 1st-order scheme and switch to the 2nd-order scheme, if necessary, when all strong initial transients have been eliminated.
    • Verbosity (for PISO Unsteady)—specify the amount of feedback directed to the Output window. The available options are None, Low, High, and Diagnostics.
  2. To improve convergence, select the Solvers > Segregated Flow node and set one or all of the following properties:
    • Enable Enhanced Stability Treatment—activate this property to increase the robustness of the segregated solver on poor-quality meshes.
    • Under-Relaxation Factor on the Velocity and Pressure child nodes—under-relax the changes of the solution during the iterative process to promote convergence. For more information, see Segregated Flow Guidelines—Under-Relaxation Factors.