NavierStokesSolver

absolute_tolerance

The absolute_tolerance is the primary convergence metric for steady cases. At least 5 orders of magnitude reduction is recommended for all residual values. The absolute_tolerance can also be used for unsteady cases, but is less meaningful than the relative_tolerance, as the initial residual values change between different physical steps.

relative_tolerance

The relative residual is defined as the ratio of the current pseudoStep’s residual to the maximum residual present in the first 10 pseudoSteps within the current physicalStep. When running unsteady cases, the relative_tolerance is typically set to 1e-2 or 1e-3. Once the nonlinear residuals drop by 2 or 3 orders of magnitude, the solver will continue to the next physicalStep. The relative_tolerance is ignored for steady cases.

kappa_MUSCL

The default value of -1 leads to a second-order upwind scheme, which is the most stable. A value of 0.33 leads to a blended upwind/central scheme, which is recommended for low subsonic flows to reduce dissipation. Values greater than 0.33 are not recommended and a value of 1 leads to an unstable scheme.

order_of_accuracy

The order_of_accuracy determines whether the solver will use 1st or 2nd order spatial discretization. The 1st order solver is faster, cheaper and most importantly, it is more dissipative, making it less likely to diverge. However, such numerical dissipation may also significantly impact the accuracy of the solution.

When initializing the flow field for unsteady cases with rotating components, such as simulating a rotor enclosed in a sliding interface, the user may need to run the 1st-order solver for around 1 or 2 revolutions. Once the flow field has been initialized, the user can fork the first-order case and switch order_of_accuracy from 1 to 2 for the child cases.

While adjusting the order_of_accuracy for the NavierStokesSolver, the TurbulenceModelSolver should also be adjusted.

The recommended time_stepping is slightly different for the 1st and 2nd order cases. For more details, see Rotational Angle per Step, maxPseudoSteps and CFL

Limiters

If the case is transonic or supersonic, the user should set limit_velocity and limit_pressure_density as TRUE in the NavierStokesSolver class.

linear_solver

linear_solver controls the configuration for the linear solver. It includes information max_iterations which specifies the number of linear iteration performed in each pseudo-step. Typically, max_iterations is set to 25~35 for the NS solver. The user might need to increase it to 50-55 if the linear residual reduction ratio after linear solver is not enough. The default max_iterations for NS solver is 30.

update_jacobian_frequency

The default value for update_jacobian_frequency is 4, which means that the Jacobian for evaluating the NS equation is updated every 4 pseudo-steps. For some challenging cases, reducing update_jacobian_frequency from 4 to 1 may help, however, this may slow the NS solver by up to approximately 30%.

equation_evaluation_frequency

The default value for equation_evaluation_frequency is 1, which means that the Navier-Stokes solution is updated every pseudo-step. For loosely-coupled simulations, the equation_evaluation_frequency value can be changed to introduce a solution update at a different frequency than the turbulence/transition model solvers. The recommended value for this parameter is 1 for a large majority of simulations.

numerical_dissipation_factor

The low-dissipation Roe scheme in Flow360 is a modification of the Roe scheme designed to address low Mach number problems and achieve reduced numerical dissipation in the range of higher-resolved wave numbers.

For steady simulations with the low-dissipation scheme, it is strongly recommend NOT to use Ramp CFL and use adaptive CFL instead due to divergence issue. For flow conditions with low Mach numbers and low Reynolds numbers, it is more effective.

The low-dissipation parameter determines the reduction in numerical flux dissipation. The recommended value for this parameter is 0.2. However, to achieve better convergence, a value of 0.5 can be used.

The solver setup parameters for the low-dissipation feature are described below.

Solver setup recommendation for the low-dissipation scheme

The following recommendations are provided to assist in running simulations with the low-dissipation scheme:

• It is recommended to first run a steady or unsteady simulation, and from that solution, start a simulation with the low-dissipation scheme.

• It is recommended to achieve a two-order-of-magnitude reduction in nonlinear residuals and keep the linear residual below 5 when running a simulation with the low-dissipation scheme. To achieve this, the step_size can be halved. Additionally, it is advisable to slightly increase the Unsteady.max_pseudo_steps / Steady.max_steps, and max_iterations parameter in the linear_solver.

• Since the low-dissipation scheme contributes to high-fidelity simulation, it is recommended to use a second-order spatial discretization with the low-dissipation scheme by setting the order_of_accuracy to 2 for both the Navier-Stokes and turbulence solvers. Alternatively, the first-order option can be used to initially march in time and space and create a well-developed initial solution before switching to the second-order scheme. This is beneficial when the flow field needs to be fully developed throughout the domain in an unsteady simulation.

• To achieve accuracy between 2nd and 3rd order in the solution, it is recommended to use a value of 1/3 for kappa_MUSCL with the low-dissipation scheme.

• In the case of poor convergence, the numerical_dissipation_factor can be increased to 0.5 or a value higher than that. Additionally, when facing such issues, setting the kappa_MUSCL parameter to -1 may also be helpful.

• It is recommended to use a value of 1 for the update_jacobian_frequency with the low-dissipation scheme.

• For CFL ramping when using the low-dissipation scheme, it is recommended to set a high value (such as 1e+5) for the CFL number and set the ramp_steps to 1. Both the initial and final CFL values can be set to the same number to keep the CFL number fixed. By using a high fixed CFL number and a small step_size, the required values for max_pseudo_steps and max_iterations can be reduced to meet the convergence criteria.

• In the case of divergence, it is recommended to reduce the step_size by half until the divergence issue is resolved.