|
SOLVER-STAGES [RESTART_STAGES] [STEP stage_name SOLVER [solver_name] [SET SOLVER_STEPS [TO] nSteps] [SET TIME_LEVELS [TO] ntlvls] [SET CYCLES [TO] numcyc] [SET {ITERATIONS [PER] [CYCLE] | ITER_CYCLE} [TO] niters [zone_selector]] [SET CFL [TO] cfl1 [zone_selector]] [SET TVD [TO] factor [zone_selector]] [SET ALPHA [TO] alpha] [SET BETA [TO] beta] [SET SEQUENCE [TO] iseq jseq kseq [zone_selector]] [SET TURBULENCE [TO] {EULER | LAMINAR} [zone_selector]] [SET IMPLICIT [TO] NONE [zone_selector]] [SET RHS [TO] scheme [order [modifier]] [ZONE zone_selector]] ENDSOLVER ENDSTEP] ENDSOLVER-STAGES |
This keyword block is used to define input for a staged solution. In a staged solution, changes can be made to various input options that would otherwise require a stopping and restarting the solution.
The various elements of the SOLVER-STAGES keyword block are
defined as follows:
|
SOLVER-STAGES ... ENDSOLVER-STAGES |
The SOLVER-STAGES and ENDSOLVER-STAGES keywords
define the beginning and end of the SOLVER-STAGES block.
| RESTART_STAGES |
This keyword should be used when restarting a staged solution.
The solution will continue with the stage in effect at the end of the
previous run.
|
STEP stage_name ... ENDSTEP |
The STEP/ENDSTEP keywords bracket input for a single stage,
where stage_name is the user-specified name for the stage.
Multiple stages are defined by using multiple STEP/ENDSTEP
sections.
|
SOLVER [solver_name] ... ENDSOLVER |
The SOLVER/ENDSOLVER keywords bracket input for a particular
solver in the current stage, where solver_name is the name of the
solver to be used.
The default, and only valid solver name in Wind-US, is
NAVIER-STOKES.
Note that the SOLVER/ENDSOLVER keywords must be specified.
| SET SOLVER_STEPS [TO] nSteps |
Specifies the number of times the current solver should be run in the
current stage.
The default is 1.
| SET TIME_LEVELS [TO] ntlvls |
Specifies the number of global time levels to advance.
The default is the value specified with the
TEMPORAL keyword block,
or the obsolete
NEWTON keyword.
If Newton iteration or dual time stepping are not being used,
this keyword should not be specified, and ntlvls will
be automatically set to 1.
| SET CYCLES [TO] numcyc |
Specifies the number of cycles to run.
The default is the value specified with the
CYCLES keyword.
| SET {ITERATIONS [PER] [CYCLE] | ITER_CYCLE} [TO] niters [zone_selector] |
Specifies the number of iterations per cycle.
The default is the value specified with the
ITERATIONS keyword.
| SET CFL [TO] cfl1 [zone_selector] |
Specifies the CFL number, time step, or time step parameter to be used.
The default is the value specified with the
CFL keyword.
Note that the options and values specified with the CFL keyword,
in particular the MODE option and the choice between CFL
and SECONDS, are still relevant for the current stage, even if
a different value is specified here for cfl1.
Note also that if MODE 2 is used with the CFL keyword,
it should only be used at the start of the run, and SET CFL
shouldn't be specified in the SOLVER-STAGES block for the
first stage.
| SET TVD [TO] factor [zone_selector] |
Specifies the TVD factor to be used.
The default is the value specified with the
TVD keyword.
Note that the type of TVD limiter (for structured grids) or slope
limiter (for unstructured grids) is controlled by the options used with
the TVD keyword, even if a different value is specified here
for factor.
|
SET ALPHA [TO] alpha SET BETA [TO] beta |
Specifies the freestream angles of attack and sideslip, in degrees.
The defaults are the values specified with the
FREESTREAM keyword.
| SET SEQUENCE [TO] iseq jseq kseq [zone_selector] |
Specifies the number of grid sequencing levels to be used in the i, j, and k directions. The defaults are the values specified with the SEQUENCE keyword. This keyword is only applicable to structured grids.
Some issues have been reported when changing grid sequencing
within solver stages. Until these can be resolved, users are advised
not to alter the grid sequencing between solver stages.
| SET TURBULENCE [TO] {EULER | LAMINAR} [zone_selector] |
The SET TURBULENCE keyword may be used to specify Euler (i.e.,
inviscid) or laminar flow.
It cannot currently be used to specify a particular turbulence model.
For turbulent flow, the model to be used must be specified using the
TURBULENCE keyword.
| SET IMPLICIT [TO] NONE [zone_selector] |
Turns off the implicit operator (i.e., switches to an explicit scheme).
This keyword only applies to unstructured grids.
| SET RHS [TO] scheme [order [modifier]] [ZONE zone_selector] |
Specifies the explicit operator to be used. The choices for scheme, order, and modifier are described in the RHS keyword documentation. Note that modifier only applies to structured grids. The default is the operator specified with the RHS keyword.
The zone specification is optional. If used, it must be preceded by the ZONE keyword.
Last updated 1 Apr 2016