Setting Parameters for the Coupled Approach

Here, you set the model and solver parameters for the coupled approach. With the coupled approach, the system of conservation equations is solved using a pseudo-time-marching method.

To set the parameters for the coupled approach:
  1. Select the Continua > [physics continuum] > Coupled Flow node and set the following model parameters:
    • Discretization—select one of the following discretization schemes for the convective and diffusive fluxes:
      • 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.

    • Integration—set one of the following pseudo-time integration schemes:
      • Implicit—set this scheme if the time scales of the phenomena of interest are either of the following:
        • The same order as the convection and/or diffusion processes (for example, vortex shedding).
        • Related to some relatively low frequency external excitation (for example, time-varying boundary conditions or boundary motion).

        This option is not available for simulations that use the Explicit Unsteady time model.

      • Explicit—set this scheme if the unsteady time scales are of the order of the acoustic processes (for example, shock front tracking).

      For more information, see (Pseudo-) Time-Marching Approach.

    • Coupled Inviscid Flux—for flows involving high supersonic and/or hypersonic regimes (Mach number of around 3 and above), set the AUSM+FVS scheme.

      For more information, see Evaluation of Inviscid Fluxes.

  2. Set the solver parameters for the coupled approach depending on the selected Time model as follows:
    • For the Steady time model, the solution in each cell is advanced independently with an optimal pseudo-time step determined locally from a specified Courant number (CFL).

      Depending on the pseudo-time integration scheme selected in Step 1, you set the CFL number using one of the following procedures:

      Integration Steps
      Implicit
      1. Select the Solvers > Coupled Implicit node and set CFL Control Method to one of the following options:
        • Automatic—adjusts the CFL number in response to AMG solver convergence behavior to maintain the specified target number of cycles. It targets a balance between the cost of forming the linear system and the cost of solving it.

          This is the default option and suitable for most simulations.

        • Expert Driver—select this option to activate the Expert Driver, an automatic convergence control tool for steady-state simulations.

        • Constant—select this option to specify a constant CFL number using the Coupled Implicit > Constant CFL node. The default Courant number is 50.
        • Linear Ramp—select this option to apply a linear ramping to the Courant number in order to help solution convergence.

          To set up the ramp, select the Coupled Implicit > Linear Ramp CFL node and set the following properties:

          • Target CFL
          • Initial CFL
          • Start Iteration
          • End Iteration

          Example: If the specified Target CFL is 50, Initial CFL is 1, Start Iteration is 100, and End Iteration is 1000, then Simcenter STAR-CCM+ uses a Courant number of 1 for iterations before 100, a Courant number of 50 for iterations after 1000, and a linearly growing Courant number between 100 and 1000 iterations.

        For more information, see Coupled Flow Solvers Reference—Coupled Implicit.

      2. To speed up the computation for cases where mass-balance convergence is slow:
        1. Select the Coupled Implicit > Convergence Accelerator node and set Convergence Accelerators to Continuity Convergence Accelerator (CCA).
        2. Select the Convergence Accelerators > Continuity Convergence Accelerator node and set the following properties:
          • Under-Relaxation Factor: tune this value for the specific flow problem. For difficult problems with stiff numerics, values as low as 0.01 or lower can be used to allow CCA to smoothly correct or reduce the remainder of the continuity equation residual. If the values for the CCA under-relaxation factor are too large for a model, the result can be strong solution oscillations, lack of convergence, or even divergence. In these cases, reduce the CCA under-relaxation factor tenfold and restart the simulation.
          • Enhanced Stability Treatment: activate this option for cases where the Coupled Implicit solver with CCA shows poor convergence.

          For more information, see Convergence Accelerator and Coupled Flow Solvers Reference—Convergence Accelerator.
      Explicit
      1. Select the Solvers > Coupled Explicit node and set Courant Number to a constant value.

        The default Courant number is 1. However, for a steady-state simulation, a value of 2 can often be used with Residual Smoothing Iterations set to 2.

      2. To help the solution convergence, you can apply a linear ramping to the Courant number:
        1. Select the Coupled Explicit > Courant Number Ramp node and set Method to Linear Ramp.
        2. Select the Courant Number Ramp > Linear Ramp node and set the following properties:
          • Start Iteration
          • End Iteration.
          • Initial Value
          Example: If the specified Courant Number is 1, Start Iteration is 100, End Iteration is 1000, and Initial Value is 0.1, then Simcenter STAR-CCM+ uses a Courant number of 0.1 for iterations before 100, a Courant number of 1 for iterations after 1000, and a linearly growing Courant number between 100 and 1000 iterations.

      For more information, see Coupled Flow Solvers Reference—Coupled Explicit.
    • For the Implicit Unsteady time model, you specify a CFL number and a physical time-step size. At each time-step, the integration scheme marches through inner iterations using optimal local pseudo-time steps that are determined from the CFL number.

      To set these solver parameters:

      1. Depending on the chosen pseudo-time Integration scheme, set the CFL number for the pseudo-time step as described for steady-state simulations.
      2. Select the Solvers > Implicit 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 CFL 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.
        • Temporal Discretization—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.
    • For the Explicit Unsteady time model, you specify a CFL number, but you are not required to specify a physical time-step size.

      Explicit time-stepping for transient simulations corresponds to the explicit pseudo time-stepping scheme for steady-state simulations. The chosen time-step is the minimum local time-step over all the fluid cells in the model, and is equal to the minimum value of the pseudo time-step in the domain.

      To set the CFL number for the time-step calculation, select the Solvers > Explicit Unsteady node and set the CFL as described for steady-state simulations.

For more information, see Coupled Flow Guidelines—Setup Recommendations.