Description

OPENFOAM_DATA Parse and convert fea struct OpenFOAM data options.

[ OPT ] = OPENFOAM_DATA( FEA, VARARGIN ) Parse and convert fea struct OpenFOAM data options. Accepts the following property/value pairs.

Property       Value/{Default}        Description
-----------------------------------------------------------------------------------
application    string {simpleFoam}    OpenFOAM solver application to run
                                        simpleFoam, pimpleFoam, rhoCentralFoam,
                                        sonicFoam, buoyantBoussinesqSimple/PimpleFoam,
                                        chtMultiRegion(Simple)Foam
ddtSchemes     string {steadyState}   Time stepping scheme
                                        steady state - steadyState, euler, localEuler
                                        time dependent - backward, CrankNicolson
tolres         scalar {1e-4/U, 1e-2/p}/vector   Stopping criteria for residuals
startTime      scalar {0.0}           Simulation start time
endTime        scalar {1000.0}        Simulation end time
deltaT         scalar {1.0}           Time step size
adjustTimeStep string no/{yes}        Adjust time step according to max Courant number in transient simulation
maxCo          scalar {0.2}           Maximum Courant number
maxDi          scalar {10.0}          Maximum Diffusion number (only for cht)
maxDeltaT      scalar {1.0}           Maximum time step size
upwind         string {linearUpwind}  Discretization scheme (div), valid options are
                                        linear, LUST, linearUpwind, limitedLinear, upwind
bound          scalar {2}             Bounding/limiting, >0 bound div, >1 bound grad
ortho          scalar {0.33}          Correction for grid non-orthogonality
writeControl   string {adjustableRunTime}  Controls the timing of write output to file
writeInterval  scalar {endTime}       Solution output write interval
purgeWrite     scalar {0/1 steady}    Specified number of output solutions
writePrecision scalar {8}             Output file write precision
timePrecision  scalar {6}             Time format precision
transportModel string {Newtonian}     Transport model
simulationType string {laminar}       Simulation type laminar, RAS, or LES
RASModel       string {kEpsilon}      RAS turbulence model kEpsilon, realizableKE
                                   RNGkEpsilon, kOmega, kOmegaSST, SpalartAllmaras
LESModel       string {Smagorinsky}   LES turbulence model
turb           struct                 Turbulence data struct fields
                                           model, inlet [k,e/o], wallfcn [1/0]
init           scalar {[]}            Initial values   []~ use init expressions
                                           i~ use solution i -1~ potential flow

TURB is a struct with fields, turb.model indicating turbulence model (kEpsilon, realizableKE RNGkEpsilon, kOmega, kOmegaSST, or SpalartAllmaras), turb.inlet a vector with two components specifying the inlet values k/epsilon or k/omega when using the corresponding models (can also be computed using the turbulence_inletbccalc function), and turb.wallfcn is a logical flag designating if turbulent wall functions should be used.

INIT by default takes the initial value expressions from the physics modes. It can also be overridden to select a previous solution (integer init = i specifies the solution number), or use potentialFoam to compute the initial values (init = -1).

In addition to the specified property value pairs. OpenFOAM dictionary properties can be set and defined by specifying a cell array with value. For example

openfoam_dict( {'system','fvSolution','solvers','p','solver'}, 'GAMG' )

sets the dict.system.fvSolution.solvers.p.solver field to GAMG. Furthermore, a n by 2 cell array value, such as for system.fvSchemes.divSchemes, can be used to assign several properties to a corresponding dictionary field.

See also: openfoam, openfoam_data_def_opt