About Coupled Solving Versus Segregated Solving

As part of the fluid physics specification, you can define whether the app solves the Navier-Stokes equations using a coupled solver or a segregated solver. The coupled solver solves the equations as a single system, enabling you to reach a solution more quickly by solving all governing equations simultaneously. The segregated solver solves each individual momentum equation as a separate scalar supplemented by the pressure equation.

See Also
Defining the Fluid Physics of a Flow Simulation

Table 1 provides a brief overview of the advantages of each solver type.

Table 1. Advantages of Coupled and Segregated Solving
Coupled Solving Segregated Solving
Converges more quickly with greater robustness and a mesh-independent convergence rate Requires half as much memory
Better suited to compressible flows Supports all boundary conditions
Often significantly more efficient computationally than segregated approach Converges nearly as fast as coupled solver for simulations where turbulence lags behind
Can simulate strongly shocked flows Can be more effective for smaller problems with auto-relaxation specified

You can reach convergence for your simulation more quickly with the coupled solver than with the segregated solver. The coupled solver, however, typically requires twice as much memory (in general, 6-7Gb of memory per one million elements). The coupled solver also does not support simulations that use the flow-split outlet boundary condition, and in general, you should not use the coupled solver for simulations with transient flow. While it is possible to simulate transient cases using the coupled solver, the smaller time steps required for time accuracy can negate any advantage that the coupled solver offers. The segregated solver is often more appropriate for simulations with transient behavior.

The coupled solver is more appropriate for steady-state simulations discretized on fine meshes because the convergence rate of the segregated solver often deteriorates markedly with increasing mesh resolution. This deterioration is especially true for compressible flow cases where auto-relaxation is not effective in accelerating the segregated solver. For shocked flows, the coupled solver is more appropriate than solving the equations individually.

When you enable the coupled solver, you can also adjust the maximum CFL and URL parameters to control how aggressively the solver iteration advances in each individual step. The suggested values depend on the presence of initial conditions and the type of flow:

  • If your simulation includes a set of well-defined initial conditions, increasing the maximum CFL usually provides faster convergence.
  • If well-defined initial conditions are not available and your analysis simulates external flows, you should decrease the CFL value to 50-100 and the URF value to 0.7 to achieve convergence.
  • If well-defined initial conditions are not available and your analysis simulates internal flows, you should decrease the CFL value even further, and you should reduce the linear convergence limit of the step to a value under 0.01.