Node146 - CFD SUPPORT

Next: Model setting without an Up: Alternative formulation Previous: Alternative formulation Contents Index

File blockMeshDict

Let us go through the file:
# less $FOAM_RUN/icoFoam/cavity/constant/polyMesh/blockMeshDict

/*--------------------------------*- 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       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Header of OpenFOAM file
```
convertToMeters 0.1;
```

Parameter convertToMeters allows the whole mesh scaling

vertices        
(
    (0 0 0)
    (1 0 0)
    (1 1 0)
    (0 1 0)
    (0 0 0.1)
    (1 0 0.1)
    (1 1 0.1)
    (0 1 0.1)
);

In section vertices there are written coordinates (points) of blocks of the mesh

blocks          
(
    hex (0 1 2 3 4 5 6 7) (20 20 1) simpleGrading (1 1 1)
);

In section blocks there are defined all blocks of the mesh; hex(0 1 2 3 4 5 6 7) (20 20 1) means hexahedral of eight vertices (0-7) according to order in vertices. The block is divided into 20 x 20 x 1 cells
Parameter simpleGrading allows refinement setting in directions (x y z)
(1 1 1) = means uniform distribution in all directions
```
edges           
(
);
```
In section edges there are defined edges connecting block vertices

If not specified otherwise, blockMesh uses lines

boundary
(
    movingWall
    {
        type wall;
        faces
        (
            (3 7 6 2)
        );
    }
    fixedWalls
    {
        type wall;
        faces
        (
            (0 4 7 3)
            (2 6 5 1)
            (1 5 4 0)
        );
    }
    frontAndBack
    {
        type empty;
        faces
        (
            (0 3 2 1)
            (4 5 6 7)
        );
    }
);

In section patches there are defined types of boundaries

mergePatchPairs 
(
);

// ************************************************************************* //

In section mergePatchPairs there are defined boundaries to be merged

Basic types of boundaries in OpenFOAM are shown in following table:

boundary type	purpose
patch	general boundary
symmetryPlane	symmetry
empty	empty, useful for 2D computations
wedge	axis symmetry
cyclic	cyclic (periodic) boundary
wall	wall
processor	inter-processor boundary (parallel computations)

OpenFOAM Training by CFD Support, CFD SUPPORT, info@cfdsupport.com +420 212 243 883 © CFD support, s.r.o., Sokolovská 270/201, 190 00 Praha 9, Czech Republic