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, 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