OpenFOAM v13 User Guide

[version 13][version 12][version 11][version 10][version 9][version 8][version 7][version 6]

[chapter contents][previous topic][next topic][index]

5.6 Mesh Zones

This section describes mesh zones and some popular tools which use zones as part of the meshing process. A zone is a list (or collection) of points or faces or cells within a mesh which is identiﬁable by a name. The list contains exclusively the indices of points, faces or cells, meaning there are three types of zone, represented in OpenFOAM by the classes pointZone , faceZone and cellZone . A unique name is required for each zone of a particular type, but the same name can be used for one pointZone, faceZone and cellZone.

A cellZone has many uses. One example is that it can deﬁne a region of the mesh to which a source term, e.g. a heat source, can be applied using an fvModel. Another is to represent a region of a mesh over which some quantity is calculated, e.g. the average temperature. A cellZone is often used to identify cells for some kind of modiﬁcation, e.g. reﬁnement, within a mesh generation process.

A faceZone can optionally include information about the orientation of the faces, in addition to their indices. The information is contained in a ﬂipMap , whose purpose is to provide a consistent orientation for all faces, e.g. to make all faces “point” in a downstream direction. The ﬂipMap contains a boolean (true/false) for each face. The sign ( $\text{[math]}$ / $\text{[math]}$ ) of normal vectors of faces marked true can then be ﬂipped so that they are oriented in a consistent direction with normal vectors of faces marked false.

A pointZone is much less commonly used that a cellZone and faceZone. It is generally used for a prescribed mesh motion, in which some or all points in a mesh are re-positioned.

5.6.1 Creating zones

A zone can be created in two ways. First, it can be created as part of the meshing process, when the zone is included within the mesh within a relevant ﬁle in the polyMesh directory. The relevant ﬁles are cellZones , faceZones and pointZones , which can each contain a set of one or more zones (in fact, a ﬁle can exist but contain zero zones).

These “static” zones can be created by a mesh generation tool, e.g. blockMesh or snappyHexMesh. Other utilities can also create them, especially the dedicated createZones tool, where the zones are conﬁgured through a createZonesDict ﬁle.

A zone can also be generated “dynamically” within an application, especially during a CFD simulation itself, i.e. within foamRun or foamMultiRun. These zones usually remain unchanged, following their generation at the beginning of a simulation. Alternatively, if a zone represents a ﬁxed region of space, and the mesh is moving, the list of indices describing a zone can be updated dynamically during a simulation.

Dynamic zones are conﬁgured through a zonesGenerator ﬁle. The ﬁle can both include the conﬁguration of new zones and may also involve “static” zones which have already been created as part of the mesh.

5.6.2 Zone generators

Zones can be conﬁgured in a zonesGenerator ﬁle, createZonesDict ﬁle and other conﬁguration ﬁles for utilities described in following sections. There are several types of zoneGenerator, which are listed in this section. For detailed information about their conﬁguration, the user can simply run the foamInfo script, e.g.

foamInfo union

Zones are always updated when there are topological changes within the mesh, e.g. meshing reﬁnement and unreﬁnement. When the mesh moves, users have the option to retain the same elements (cells, faces, points) within the zone, such that the zone moves with the mesh. Alternatively, they can update the elements of a zone during a simulation by setting the moveUpdate switch to on/yes/true. This allows the zones to represent regions ﬁxed in space with the mesh moving within it.

The ﬁrst set of zone generators describe volume regions within the domain. They can create a zone of cells, faces or points contained within the volume region. Cells and faces are included when their centres are within the volume; points are included which are within the volume. The volume zone generators are listed below.

annulus : selects cells, faces or points inside an annulus.
box : selects cells, faces or points inside a box.
cylinder : selects cells, faces or points inside a cylinder.
hemisphere : selects cells, faces or points inside a hemisphere.
insideSurface : selects cells, faces or points inside a closed surface described by a surface geometry ﬁle, e.g. surface.obj.
sphere : selects cells, faces or points inside a sphere.
truncatedCone : selects cells, faces or points inside a truncated cone.

An example conﬁguration of a hemisphere zone generator is presented below (taking from running “foamInfo hemisphere”).

hemisphere1
{
    type        hemisphere;
    zoneType    cell;

    centre      (-0.001 0.001 0);
    axis        (0 1 0);
    radius      0.001;
}

There are then zone generators which are speciﬁc to cells, faces and points. The biggest set of these is the zone generators for faces which are listed below.

face : creates a face zone from point, cell and face zones provided by a list of zoneGenerators.
flip : inverts the flipMap of a face zone from a given zoneGenerator.
normal : selects faces from a given zoneGenerator that are aligned with a speciﬁed normal direction.
orient : sets the face orientation flipMap of a face zone.
patch : creates a face zone from a set of patches.
plane : creates a face zone from faces, whose vector connecting its adjacent cell centres, intersects a speciﬁed plane.
surface : creates a face zone from faces whose vector, , whose vector connecting its adjacent cell centres, intersects a surface geometry, e.g. surface.obj.

As discussed in the introduction to this section, a face zone can optionally include a flipMap . A flipMap is required, for example, to calculate the ﬂow rate through an area described by a face zone by summing the ﬂuxes $\text{[math]}$ on all the faces in the face zone. That calculation is only meaningful if the face area vectors, used to calculate $\text{[math]}$ , point in a consistent direction. To ensure consistency, the sign of $\text{[math]}$ is inverted for faces marked true in the flipMap.

Speciﬁc cell and point zone generators are listed below.

cellZone : selects and/or generates a cell zone for a tool that requires one, e.g. a functionObject, fvModel, fvConstraint or utility application.
containsPoints: creates a cell zone containing the speciﬁed points.
point: creates a point zone from face, cell and point zones provided by list of zoneGenerators.

The ﬁnal set of zone generators create, that manipulate and combine zones, are listed below. When used to create a face zone, they have speciﬁc rules about creating a flipMap.

all : creates a zone using all cells, faces or points of the mesh; no flipMap for a face zone.
clear : clears all zones from a mesh.
difference : selects cell, face or point elements in the ﬁrst speciﬁed zone and removes the elements in subsequent speciﬁed zones.
intersection : selects cell, face or point elements common to all the speciﬁed zones; can contain a flipMap if one face zone includes one.
invert : selects cell, face or point elements in the mesh and removes the elements from the speciﬁed zones.
periodic : activates a speciﬁed set of zones for a given period with optional repetition.
remove : removes speciﬁed zones from a mesh.
set : converts a legacy cell, face or point set to an equivalent zone; no flipMap a the face zone.
union : selects all cell, face or point elements from all the speciﬁed zones; can contain a flipMap if all face zones include one.
write : writes existing zones to the mesh, e.g. for visualisation.

5.6.3 The createZones utility

The createZones utility creates “static” zones that form part of a mesh. There are many example cases in OpenFOAM that use createZones that can be inspected to learn about its use. One example is the coolingSphere case (in $FOAM_TUTORIALS/multiRegion/CHT) which generates a cell zone that is subsequently used to form a separate mesh region for a solid sphere. The conﬁguration from the createPatchDict ﬁle is shown below.

16solid

17{

18    type        sphere;

19    zoneType    cell;

20

21    centre      (0 0 0);

22    radius      $blockMeshDict!geometry/sphere/radius;

23}

24

25// ************************************************************************* //

It generates a zone named solid using the sphere zone generator. The zone type is a cell zone. The remaining parameters describe the sphere, namely the centre and radius. The latter is read from the blockMeshDict ﬁle using a macro expansion, described in section 4.2.10 .

The mesh and cell zone are generated by running blockMesh and createZones respectively. blockMesh ﬁrst produces the standard mesh ﬁles in the constant/polyMesh. createZones then generates an additional cellZones ﬁle in that directory, containing the list of cell indices that make up the zone.

5.6.4 The reﬁneMesh utility

The reﬁneMesh utility reﬁnes cells in a mesh. The reﬁnement can be applied to cells in the entire mesh or to speciﬁed regions of the mesh. The reﬁnement is applied by splitting cells, which can be applied in all three directions or on one or two speciﬁed directions.

To apply reﬁnement across the entire mesh and in all three directions, reﬁneMesh can be run using the -all option, i.e.

refineMesh -all

Otherwise, the region of the mesh and/or reﬁnement directions must be conﬁgured using a reﬁneMeshDict ﬁle.

There are many example cases in OpenFOAM which include reﬁneMeshDict ﬁles. One is the pipeCyclic case (in $FOAM_TUTORIALS/incompressibleFluid) whose reﬁneMeshDict ﬁle is shown below.

16

17hexRef8         yes;

18

19zone

20{

21    type    box;

22    box     (-1e6 -1e6 -1e6)(1e6 -0.15 0.3);

23}

24

25// ************************************************************************* //

The ﬁle includes a zone entry to describe a cell zone conﬁgured with a box zone generator. The reﬁnement is speciﬁed through the hexRef8 switch, set to on. hexRef8 reﬁnes cells in all directions, splitting each selected cell $\text{[math]}$ . It is the method used by snappyHexMesh which keeps a record of the reﬁnement history in a reﬁnementHistory ﬁle in the polyMesh directory.

The DTCHull case (in $FOAM_TUTORIALS/incompressibleVoF) is another example that uses the reﬁneMesh utility. It is a case of ship hydrodynamics which generates an initial mesh which has high aspect ratio cells, stretched in the horizontal plane, in the vicinity of the water-air interface. Before meshing the ship hull with snappyHexMesh, the aspect ratio of cells is gradually reduced from the far ﬁeld to the hull, by successive reﬁnements of cells in the horizontal directions. The reﬁneMeshDict ﬁle for this case is shown below.

16

17coordinates

18{

19    type        global;

20

21    e1          (1 0 0);

22    e2          (0 1 0);

23

24    directions  (e1 e2);

25}

26

27zones

28{

29    level1

30    {

31        type    box;

32        box     (-10 -6 -3) (10 0 3);

33    }

34

35    level2

36    {

37        type    box;

38        box     (-5 -3 -2.5) (9 0 2);

39    }

40

41    level3

42    {

43        type    box;

44        box     (-3 -1.5 -1) (8 0 1.5);

45    }

46

47    level4

48    {

49        type    box;

50        box     (-2 -1 -0.6) (7 0 1);

51    }

52

53    level5

54    {

55        type    box;

56        box     (-1 -0.6 -0.3) (6.5 0 0.8);

57    }

58

59    level6

60    {

61        type    box;

62        box     (-0.5 -0.55 -0.15) (6.25 0 0.65);

63    }

64}

65

66// ************************************************************************* //

It ﬁrst describes the reﬁnement directions by the coordinates sub-dictionary. The co-ordinates must be speciﬁed by two orthogonal directions described by the e1 and e2 vectors. The directions parameter then lists the reﬁnement directions, which could theoretically include e3, the vector calculated orthogonal to e1 and e2 (forming a right-handed set of axes).

The reﬁnement is then speciﬁed in zones described in the a zones sub-dictionary. Six box zones are listed from largest to smallest. Reﬁnement is applied successively to each zone so that it produces six levels of reﬁnement in the ﬁnal box, ﬁve levels in the region described by the ﬁfth box beyond the ﬁnal box, and so on.

5.6.5 The createPatch utility

The createPatch utility creates new patches from collections of boundary faces. It enables users to make changes to the patch conﬁguration in a mesh, often in the ﬁnal stages of a meshing workﬂow. The utility is conﬁgured by a createPatchDict ﬁle.

There are some examples in OpenFOAM which use createPatch. Most of them create a patch from faces deﬁned by a face zone. The hotRoomComfort example (in $FOAM_TUTORIALS/ﬂuid) contains a createPatchDict ﬁle which creates an inlet and an outlet patch in a mesh whose boundary initially contains a single wall patch. The createPatchDict ﬁle is given below, showing each patch is generated from a box zone.

16patches

17{

18    inlet

19    {

20        // Dictionary to construct new patch from

21        patchInfo

22        {

23            type patch;

24        }

25

26        // Construct from zone

27        constructFrom zone;

28

29        // Generate zone

30        zone

31        {

32            type        box;

33            box         (-0.001 0.25 1.1)(0.001 0.75 1.3);

34        }

35    }

36

37    outlet

38    {

39        // Dictionary to construct new patch from

40        patchInfo

41        {

42            type patch;

43        }

44

45        // Construct from zone

46        constructFrom zone;

47

48        // Generate zone

49        zone

50        {

51            type        box;

52            box         (1.75 2.999 0.3)(2.25 3.001 0.5);

53        }

54    }

55}

56

57// ************************************************************************* //

The potentialFreeSurfaceMovingOscillatingBox case (in $FOAM_TUTORIALS/isothermalFluid) uses the createPatchDict shown below.

16patches

17{

18    floatingObjectBottom

19    {

20        // Dictionary to construct new patch from

21        patchInfo

22        {

23            type wall;

24        }

25

26        // Construct patch from a faceZone

27        constructFrom zone;

28

29        zone

30        {

31            type        normal;

32

33            normal      (0 1 0);

34            tol         0.01;

35

36            floatingObject

37            {

38                type        patch;

39                patch       floatingObject;

40            }

41        }

42    }

43}

44

45// ************************************************************************* //

This example uses a normal zone generator applied to a zone generated from patch. The patch zone generation is conﬁgured within the normal zone conﬁguration, resulting in a zone containing faces, oriented with the speciﬁed normal direction, that are extracted from the patch.

5.6.6 The subsetMesh utility

The subsetMesh utility creates a new mesh which is a subset of an existing mesh. It is commonly used in a meshing workﬂow which creates a mesh, then uses subsetMesh to remove part of the mesh.

The ﬂoatingObject tutorial (in $FOAM_TUTORIALS/incompressibleVoF) provides a good example of its use. A mesh is initially created of a box-shaped domain. A ﬂoating object is then introduced corresponding to a zone conﬁgured in subsetMeshDict, shown below.

16

17zone

18{

19    type        box;

20    select      outside;

21    box         (0.35 0.35 0.1) (0.65 0.55 0.6);

22}

23

24patch   floatingObject;

25

26// ************************************************************************* //

The zone is conﬁgured by deﬁning a box with the addition of the optional selection keyword which selects cells outside the box. Consequently, the new mesh becomes the original mesh without the cells contained with the box, which represents the ﬂoating object. A patch entry provides a name for the patch formed by the faces exposed by removal of the cells.

OpenFOAM v13 User Guide - 5.6 Mesh Zones