In this section we discuss the way in which boundaries are treated in OpenFOAM. The subject of boundaries is a little involved because their role in modelling is not simply that of a geometric entity but an integral part of the solution and numerics through boundary conditions or inter-boundary ‘connections’. A discussion of boundaries sits uncomfortably between a discussion on meshes, fields, discretisation, computational processing etc. Its placement in this Chapter on meshes is a choice of convenience.
We first need to consider that, for the purpose of applying boundary conditions, a boundary is generally broken up into a set of patches. One patch may include one or more enclosed areas of the boundary surface which do not necessarily need to be physically connected.
There are three attributes associated with a patch that are described below in their natural hierarchy and Figure 5.3 shows the names of different patch types introduced at each level of the hierarchy. The hierarchy described below is very similar, but not identical, to the class hierarchy used in the OpenFOAM library.
- Base type
- The type of patch described purely in terms of geometry or a data ‘communication link’.
- Primitive type
- The base numerical patch condition assigned to a field variable on the patch.
- Derived type
- A complex patch condition, derived from the primitive type, assigned to a field variable on the patch.
The patch types are specified in the mesh and field files of a OpenFOAM case. More precisely:
- the base type is specified under the type keyword for each patch in the boundary file, located in the constant/polyMesh directory;
- the numerical patch type, be it a primitive or derived type, is specified under the type keyword for each patch in a field file.
An example boundary file is shown below for a sonicFoam case, followed by a pressure field file, p, for the same case:
22 type patch;
23 nFaces 50;
24 startFace 10325;
28 type patch;
29 nFaces 40;
30 startFace 10375;
34 type symmetryPlane;
35 inGroups 1(symmetryPlane);
36 nFaces 25;
37 startFace 10415;
41 type symmetryPlane;
42 inGroups 1(symmetryPlane);
43 nFaces 125;
44 startFace 10440;
48 type patch;
49 nFaces 110;
50 startFace 10565;
54 type empty;
55 inGroups 1(empty);
56 nFaces 10500;
57 startFace 10675;
61 // ************************************************************************* //
19 internalField uniform 1;
25 type fixedValue;
26 value uniform 1;
31 type waveTransmissive;
32 field p;
33 phi phi;
34 rho rho;
35 psi thermo:psi;
36 gamma 1.4;
37 fieldInf 1;
38 lInf 3;
39 value uniform 1;
44 type symmetryPlane;
49 type symmetryPlane;
54 type zeroGradient;
59 type empty;
63 // ************************************************************************* //
The type in the boundary file is patch for all patches except those that have some geometrical constraint applied to them, i.e. the symmetryPlane and empty patches. The p file includes primitive types applied to the inlet and bottom faces, and a more complex derived type applied to the outlet. Comparison of the two files shows that the base and numerical types are consistent where the base type is not a simple patch, i.e. for the symmetryPlane and empty patches.
The base and geometric types are described below; the keywords used for specifying these types in OpenFOAM are summarised in Table 5.1.
- The basic patch type for a patch condition that contains no geometric or topological information about the mesh (with the exception of wall), e.g. an inlet or an outlet.
- There are instances where a patch that coincides with a wall needs to be identifiable as such, particularly where specialist modelling is applied at wall boundaries. A good example is wall turbulence modelling where a wall must be specified with a wall patch type, so that the distance from the wall to the cell centres next to the wall are stored as part of the patch.
- For a symmetry plane.
- While OpenFOAM always generates geometries in 3 dimensions, it can be instructed to solve in 2 (or 1) dimensions by specifying a special empty condition on each patch whose plane is normal to the 3rd (and 2nd) dimension for which no solution is required.
- For 2 dimensional axi-symmetric cases, e.g. a cylinder, the geometry is specified as a wedge of small angle (e.g. ) and 1 cell thick running along the plane of symmetry, straddling one of the coordinate planes, as shown in Figure 5.4. The axi-symmetric wedge planes must be specified as separate patches of wedge type. The details of generating wedge-shaped geometries using blockMesh are described in section 5.3.3.
- Enables two patches to be treated as if they are physically connected; used for repeated geometries, e.g. heat exchanger tube bundles. One cyclic patch is linked to another through a neighbourPatch keyword in the boundary file. Each pair of connecting faces must have similar area to within a tolerance given by the matchTolerance keyword in the boundary file. Faces do not need to be of the same orientation.
- If a code is being run in parallel, on a number of processors, then the mesh must be divided up so that each processor computes on roughly the same number of cells. The boundaries between the different parts of the mesh are called processor boundaries.
The primitive types are listed in Table 5.2.
There are numerous derived types of boundary conditions in OpenFOAM, too many to list here. Instead a small selection is listed in Table 5.3. If the user wishes to obtain a list of all available models, they should consult the OpenFOAM source code. Derived boundary condition source code can be found at the following locations:
- in $FOAM_SRC/finiteVolume/fields/fvPatchFields/derived
- within certain model libraries, that can be located by typing the following command in a terminal window
find $FOAM_SRC -name ”*derivedFvPatch*”
- within certain solvers, that can be located by typing the following command in a terminal window
find $FOAM_SOLVERS -name ”*fvPatch*”