Next: Model setting without an Up: Alternative formulation Previous: Alternative formulation Contents Index
Boundary and Initial condition
- Initial and boundary conditions are stored in directories named with numbers
- Number in directory name stands for time layer of the solution
- Usually initial conditions are stored in directory 0
- In case of solver icoFoam one imposes pressure p and velocity U.
- It is necessary to impose initial and boundary conditions in the first time layer (typically 0 )
- Let us take a look for example at the pressure:
# cat $FOAM_RUN/icoFoam/cavity/0/p/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.2.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //dimensions [0 2 -2 0 0 0 0];
- Parameter dimensions stands for physical dimensions according to SI unit system:
SI [kg m s K mol A cd], e.g. for pressure:
(kinematic pressure)internalField uniform 0;
- Parameter internalField defines values in cell volumes of the mesh
- Values can be constant all over the flow field (uniform) with corresponding value
- Or values can be non-constant (nonuniform, i.e. possibly different value in each cell) with list of values (according to cell IDs)
boundaryField { movingWall { type zeroGradient; } fixedWalls { type zeroGradient; } frontAndBack { type empty; } } // ************************************************************************* // - boundaryField defines boundary conditions for mesh boundaries
- type defines real boundary condition
- e.g. zeroGradient is so called homogeneous Neumann boundary condition, which means that quantity gradient is zero in direction perpendicular to the boundary
- Boundary condition empty means, that there is no flow in direction perpendicular to the boundary, this boundary condition must correspond to definition in polyMesh/boundary
- Let us take a look at the velocity file :
# cat $FOAM_RUN/icoFoam/cavity/0/U/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: 2.2.1 | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volVectorField; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { movingWall { type fixedValue; value uniform (1 0 0); } fixedWalls { type fixedValue; value uniform (0 0 0); } frontAndBack { type empty; } } // ************************************************************************* // - Velocity U is a vector and has three components (Ux, Uy, Uz)
- At the wall there is often prescribed fixed value for velocity (Dirichlet boundary condition): fixedValue, which needs its value, either uniform or nonuniform
- Condition uniform (0 0 0) means the velocity is zero at the wall
- Condition uniform (1 0 0) means the velocity is 1 m/s in magnitude and points in the direction of the coordinate x axis (wall is moving)
Next: Model setting without an Up: Alternative formulation Previous: Alternative formulation Contents Index