.. _knowledge_base_navierStokesSolver: :ref:`navierStokesSolver ` ========================================================= :code:`absoluteTolerance` ------------------------- The :code:`absoluteTolerance` is the primary convergence metric for steady cases. At least 5 orders of magnitude reduction is recommended for all residual values. The :code:`absoluteTolerance` can also be used for unsteady cases, but is less meaningful than the :code:`relativeTolerance`, as the initial residual values change between different physical steps. .. _relativeTolerance: :code:`relativeTolerance` ------------------------- 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 :code:`relativeTolerance` 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 :code:`relativeTolerance` is ignored for steady cases. .. _kappaMUSCL: :code:`kappaMUSCL` ------------------ 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. .. _knowledge_base_orderOfAccuracy: :code:`orderOfAccuracy` ----------------------- The :code:`orderOfAccuracy` 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 :code:`orderOfAccuracy` from 1 to 2 for the child cases. While adjusting the :code:`orderOfAccuracy` for the :code:`navierStokesSolver`, the :ref:`turbulenceModelSolver ` should also be adjusted. The recommended :code:`timeStepping` is slightly different for the 1st and 2nd order cases. For more details, see :ref:`Rotational Angle per Step `, :ref:`maxPseudoSteps ` and :ref:`CFL ` Limiters -------- If the case is transonic or supersonic, the user should set :code:`limitVelocity` and :code:`limitPressureDensity` as :code:`TRUE` in the :ref:`Navier Stokes solver parameters` section of their input file. :code:`linearIterations` ------------------------ :code:`linearIterations` controls the number of linear iterations in each pseudo-step. Typically, :code:`linearIterations` is set to 25~35 for the NS solver. The user might need to increase it to 50-55 for challenging cases to improve convergence. :code:`updateJacobianFrequency` -------------------------------- The default value for :code:`updateJacobianFrequency` is 4, which means that the Jacobian for evaluating the NS equation is updated every 4 pseudo-steps. For some challenging cases, reducing :code:`updateJacobianFrequency` from 4 to 1 may help, however, this may slow the NS solver by up to approximately 30%. :code:`equationEvalFrequency` ------------------------------ The default value for :code:`equationEvalFrequency` is 1, which means that the Navier-Stokes solution is updated every pseudo-step. For loosely-coupled simulations, the :code:`equationEvalFrequency` 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.