Linear Solvers and Preconditioners

Linear solvers (and preconditioners) are used in implicit (pseudo)time integration schemes (any option with “IMPLICIT” or “DUAL-TIME” in the name). This page lists the available options and provides guidance on how to setup the linear solvers for best results. As the numerical properties of the linear systems vary significantly with application, and even with application-specific options, a “one size fits all” default setting is not available.

• Option List
  • Linear Solvers
  • Linear Preconditioners
  • External Solvers
• Setup Advice
  • Fluid Simulations
  • Structural Simulations
  • Mesh Deformation
  • Discrete Adjoint

Option List

Linear Solvers

The following options accept a type of linear solver:

• LINEAR_SOLVER: Main option for direct/primal and continuous adjoint problems. The linear solver used by all physics solvers of the zone associated with the configuration file.
• DISCADJ_LIN_SOLVER: Main option for discrete adjoint problems.
• DEFORM_LINEAR_SOLVER: Linear solver for elasticity-based mesh deformation.

In most applications the linear solver tolerance is defined by option LINEAR_SOLVER_ERROR, and the maximum number of iterations by LINEAR_SOLVER_ITER. Mesh deformation uses DEFORM_LINEAR_SOLVER_ERROR and DEFORM_LINEAR_SOLVER_ITER, as it may coexist with other physics in the same physical zone.

The available types of (iterative) linear solver are:

Note: The SMOOTHER option is not available for mesh deformation applications (as it stands little chance of doing any smoothing).

Linear Preconditioners

Analogously to the above options, the following accept a type of linear preconditioner:

• LINEAR_SOLVER_PREC
• DISCADJ_LIN_PREC
• DEFORM_LINEAR_SOLVER_PREC

The available types of preconditioner are:

Note: Only JACOBI and ILU are compatible with discrete adjoint solvers.

External Solvers

Version 7 introduces experimental support for the direct sparse solver PaStiX see detailed options in TestCases/pastix_support/readme.txt

Setup Advice

For tiny problems with ~10k nodes almost any solver will do, these settings are more important for medium-large problems.

Disclaimer: Your own experience is more important that this advice, but if you have yet to gain some this should help.

Fluid Simulations

Fastest overall convergence is usually obtained by using the highest CFL number for which the flow solver is stable, and the linear systems still reasonably economic to solve. For example central schemes like JST allow very high CFL values, however at some point (100-400 for RANS grids) the linear systems become too expensive to solve and performance starts decreasing. Upwind schemes are less plagued by this as stability considerations usually put a lower limit on CFL, and the linear systems are better conditioned to begin with.

Like CFL, the linear solver tolerance should be the highest (i.e. less accurate) possible for which the flow solver is still stable, usually in the 0.05-0.001 range, having to go lower is often a sign of poor mesh quality resulting in localized high residuals. A high linear tolerance does not reduce the accuracy of the final results since the solution is iterative, and on each iteration of the flow solver the right hand side of the linear system is the nonlinear residual, only this residual needs to be low for accurate solution of the discretized nonlinear equations.

The maximum number of iterations should allow the linear solver to converge, however the memory footprint of FGMRES (which should be your default solver) is proportional to that number, if that becomes a problem you can switch to RESTARTED_FGMRES or BCGSTAB, the latter may perform better for stiff systems like those resulting from central schemes at high CFL. For a typical problem with an upwind scheme 10 iterations should be sufficient, for central schemes up to 50 may be required.

High CFL cases will usually require the ILU preconditioner, while low CFL cases may run better with LU_SGS as even if more linear iterations are required, LU_SGS has no setup cost.

Finally, the concept of high/low CFL is somewhat case dependent, for RANS meshes (stretched close to walls) and upwind schemes, high is greater than 100 and low less than 20, central schemes move the limits down, time domain and less stretched meshes (e.g. for Euler or Navier-Stokes simulations) move the limits up.

Structural Simulations

At scale these become the most difficult systems to solve in SU2 due to their elliptical nature, they are easier for time-domain problems nonetheless always start with the ILU preconditioner. A much larger number of linear iterations is required (>100) RESTARTED_FGMRES or CONJUGATE_GRADIENT should therefore be used. For linear elasticity an error of at most 1e-8 should be targeted as contrary to fluid problems there are no outer iterations, for nonlinear elasticity 1e-6 may suffice as a few nonlinear iterations are required.

Note: If the solution becomes challenging, and the problem is 2D or you have RAM to spare, consider using the external direct solvers.

Mesh Deformation

For elasticity-based mesh deformation the advice is the same as for structural simulations.

Discrete Adjoint

Discrete adjoint applications respond well to high CFL values, the advice is generally the same as for the primal counterpart (fluid or structural). The ILU preconditioner should be used as JACOBI will only give an advantage for very low CFL values.

Note: For steady-state discrete adjoint problems the system matrix does not change, therefore the external direct solvers may achieve the shortest solution time for 2D and medium scale (<1M nodes) 3D problems.