Navier Stokes solver¶

Some parameters are shared between all the available velocity-pressure solvers. All the parameters in the following example have sensible defaults except for the solver type which you must set. The other parameters in the example input shown below are the default values. The possible values for solver type (IPCS-A, SIMPLE, PISO etc) are listed in the sections below with a brief description. You can also write your own solver, see Writing a custom solver.

solver:
    type: IPCS-A
    num_inner_iter: 10
    allowable_error_inner: 1.0e-4
    polynomial_degree_pressure: 1  # not needed, this is the default value
    polynomial_degree_velocity: 2  # not needed, this is the default value
    function_space_pressure: DG    # not needed, this is the default value
    function_space_velocity: DG    # not needed, this is the default value
    u:
        # see linear solver documentation below
    p:
        # see linear solver documentation below

The inner iterations (pressure correction iterations) will run a maximum of num_inner_iter times for each time step, but the iterations will exit early if the \(l^2\) error of the difference between the predicted and corrected velocity field is less than the given value allowable_error_inner.

Some control parameters exist outside the common ones shown above, but none of these are of the type that a normal user would probably need to change, so they are only documented in the source code of the individual solvers.

The following parameters are relevant for under-relaxed solver implementations (SIMPLE, PISO, PIMPLE):

relaxation_u, relaxation_p: Relaxation factors. A value of 1.0 means no relaxation, 0.0 means no update at all (pointless). A value of 0.5 means that the result is an even blend of the computed value and the previous iteration value

relaxation_u_last_iter, relaxation_p_last_iter: Some solvers will differentiate the last inner iteration from all other iterations. These parameters default to 1.0 in order to perform a “propper” update at the end of a time step with no relaxation applied.

IPCS-A¶

Incremental Pressure Correction Scheme on Algebraic form. This is an iterative Chorin/Temam type pressure correction solver.

This is the most used solver and it typically has more advanced features than the other solvers. See 2 for details.

IPCS-D¶

Incremental Pressure Correction Scheme on Differential form. This is an iterative Chorin/Temam type pressure correction solver where the pressure correction Poisson equation is assembled from an elliptic operator and not algebraicly from matrices. The divergence of the velocity field is hence not very low and the method is not so strongly recommended for DG FEM, but it is one of the most common solvers for the Navier-Stokes equations outside of DG FEM and it has a smaller numerical stencil and may be faster than the IPCS-A method. See 2 for details.

SIMPLE¶

Semi-Implicit Method for Pressure-Linked Equations. The implementation of the algorithm is based on 1. See 2 for a comparison with IPCS-A and IPCS-D.

PISO¶

The pressure correction method by Issa (1986), Pressure-Implicit with Splitting of Operators. PISO adds an additional correction step to the SIMPLE algorithm.

PIMPLE¶

A Navier-Stokes solver based on the PIMPLE algorithm as implemented in OpenFOAM and partially described in the PhD thesis of Jasak (1996; the PISO loop only).

num_pressure_corr: The number of PISO iterations for each PIMPLE loop (the number of PIMPLE loops is controlled by the standard num_inner_iter parameter).

Coupled¶

Solves the velocity-pressure saddle point block-matrix equation system coupled. Do not use this solver for large meshes. Even when using the multi-cpu distributed multi frontal MUMPS or SuperLU_dist direct solvers there is a quite small (perhaps around 1 million on a recent workstation?) limit to how many degrees of freedom can be computed. For very small examples it may be faster than using pressure-correction iterations and there is no resulting splitting error which makes it great for testing and benchmarking the split solvers.

No block-system preconditioners are available in Ocellaris for the coupled Navier-Stokes solver, so iterative linear solvers will either not converge or perhaps “converge” to nonsensical solutions. Only use with direct solvers!

Analytical¶

Use the initial condition C++ code (possibly containing the time variable t which will be updated for each time step) to define the velocity and pressure for all time steps. This can be useful for testing other parts of the Ocellaris solution framework with a known Navier-Stokes solution.

Specifying the linear solver¶

All equation systems that require global solves, like the velocity, pressure and potentially multi phase models, will have their own optional definition of the linear solver. These can be described in two ways, the simple FEniCS DOLFIN based setup where some limited configuration is possible, or the full PETSc KSP setup where all of the PETSc options are configurable plus a few options added by Ocellaris.

It is recommended to use the KSP setup. It is the default, it is more powerfull and it can do everything supported by the FEniCS DOLFIN setup. The DOLFIN setup is kept for comparison and to be able to test the exact same setup used by “normal” FEniCS codes.

PETSC KSP solver setup (use_ksp = yes)¶

This linear solver setup is used by most linear solvers inside Ocellaris. Most solvers set reasonable defaults. Use these as starting points for your own experimentations. The Ocellaris log file shows the setup which is used for the different linear solvers in your simulation.

solver:
    u:
        use_ksp: yes
        petsc_ksp_type: gmres
        petsc_pc_type: asm
        petsc_ksp_initial_guess_nonzero: yes
        inner_iter_rtol: [1.0e-15, 1.0e-15, 1.0e-15]
        inner_iter_atol: [1.0e-15, 1.0e-15, 1.0e-15]
        inner_iter_max_it: [100, 100, 100]

use_ksp: yes: Signal that we want to use the KSP solver setup (this is default in most situations).

petsc_XXXX: Any PETSc parameter. Examples: ksp_type sets the solver name and pc_type sets the preconditioner name. Look at the PETSc documentation for the full list of tunable parameters, or give petsc_help: 'ENABLED' to get a dump of possible parameters (the program will exit after giving the parameter listing).

inner_iter_control: The number of iterations and tolerances in the Krylov solver can be set for three categories of solves. The first X inner iterations (pressure correction iterations in the Navier-Stokes solver), the last Y inner iterations and the rest of the iterations (the middle number). The numbers X and Y are set by inner_iter_control: [X, Y]. The default values are X=Y=3.

inner_iter_rtol, inner_iter_atol, inner_iter_max_it: The relative and absolute tolerances in the Krylov solver (default values are typically rtol = 1.0e-10 and atol = 1.0e-15). The maximum number of Krylov iterations is by default 100 for most solvers. If the solution is not converged the procedure will just continue, it is not always necessary to fully converge when applying an iterative solver, at least not in the inner first iterations (see below note on iterations).

Note

Inner iterations refer to the main iterations inside each time step, typically pressure correction iterations (implemented in code inside Ocellaris). Krylov iterations refer to iterations inside the linear equation solver (provided by PETSc). The Krylov iterations are nested inside the inner iterations which are nested inside the time loop.

FEniCS DOLFIN solver setup (use_ksp = no)¶

solver:
    u:
        use_ksp: no
        solver: gmres
        preconditioner: additive_schwarz
        parameters:
            any_parameter_supported_by_dolfin: valid_value

use_ksp: no: Signal that we want to use the simplified setup

solver, preconditioner: The names of the preconditioner and linear solver. Any values (string) supported by FEniCS DOLFIN are supported. The default values in FEniCS are used if none are specified (bad idea for large systems)

parameters: Any parameter keys and values supported by FEniCS DOLFIN. See the DOLFIN documentation for these.

Citations

1: Benedikt Klein, Florian Kummer, Markus Keil, and Martin Oberlack. An extension of the SIMPLE based discontinuous galerkin solver to unsteady incompressible flows. International Journal for Numerical Methods in Fluids, 77(10):571–589, 2015. doi:10.1002/fld.3994.
2(1,2,3): Tormod Landet and Mikael Mortensen. On exactly incompressible DG FEM pressure splitting schemes for the Navier-Stokes equation. arXiv physics.comp-ph, 2019. arXiv:1903.11943.

Ocellaris DG FEM multiphase flow solver

Ocellaris 2019.1.0 documentation