OpenFOAM v14 User Guide

[version 14][version 13][version 12][version 11][version 10][version 9][version 8][version 7][version 6]

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

6.3 Introduction to boundary conditions

Boundary conditions are speciﬁed in ﬁeld ﬁles, e.g. p, U, in time directories. The structure of these ﬁles is introduced in sections 2.1.4 and 4.2.9 , with the keyword entries dimensions, internalField, boundaryField, and, optionally sources. The boundaryField sub-dictionary is the place where boundary conditions are speciﬁed. An entry for each patch in the mesh, which are speciﬁed in the boundary ﬁle; below is a sample ﬁle from a 2D incompressibleFluid example in OpenFOAM.

5
(
    outlet
    {
        type            patch;
        nFaces          320;
        startFace       198740;
    }
    up
    {
        type            symmetry;
        inGroups        List<word> 1(symmetry);
        nFaces          760;
        startFace       199060;
    }
    hole
    {
        type            wall;
        inGroups        List<word> 1(wall);
        nFaces          1120;
        startFace       199820;
    }
    frontAndBack
    {
        type            empty;
        inGroups        List<word> 1(empty);
        nFaces          200000;
        startFace       200940;
    }
    inlet
    {
        type            patch;
        nFaces          320;
        startFace       400940;
    }
)

The corresponding pressure ﬁeld ﬁle, p, is shown below.

16

17dimensions      [kinematicPressure];

18

19internalField   uniform 0;

20

21boundaryField

22{

23    inlet

24    {

25       type             zeroGradient;

26    }

27    outlet

28    {

29        type            fixedValue;

30        value           uniform 0;

31    }

32    up

33    {

34        type            symmetry;

35    }

36    hole

37    {

38        type            zeroGradient;

39    }

40    frontAndBack

41    {

42        type            empty;

43    }

44}

45

46// ************************************************************************* //

Each entry in the boundaryField sub-dictionary must include a type entry which speciﬁes the type of boundary condition. The examples above include zeroGradient and ﬁxedValue conditions corresponding to generic patches deﬁned in the boundary ﬁle. They also include symmetry and empty types corresponding to equivalent constraint patches, e.g. the up patch is deﬁned as symmetry in the mesh and uses a symmetry condition in the ﬁeld ﬁle.

For details about the main boundary conditions used in OpenFOAM, refer to Chapter 4 of Notes on Computational Fluid Dynamics: General Principles.

6.3.1 Patch selection in ﬁeld ﬁles

There are three diﬀerent ways an entry can be speciﬁed for a patch in the boundaryField of a ﬁeld ﬁle: 1) by patch name; 2) by group name; 3) matching a patch name with a regular expression. They are listed here in order of precedence which is obeyed if multiple entries are valid of a particular patch. The diﬀerent speciﬁcations can be illustrated by imagining a mesh with the following patches.

inlet: a generic patch.
lowerWall and upperWall: two wall patches.
outletSmall, outletMedium and outletLarge: three outlet patches of generic type, all in a patch group named outlet.

Then imagine the following boundaryField for a ﬁeld, e.g. p, corresponding to the patches above.

boundaryField
{
    inlet
    {
       type             zeroGradient;
    }
    ".*Wall"
    {
        type            zeroGradient;
    }
    outletSmall
    {
        type            fixedValue;
        value           uniform 1;
    }
    outlet
    {
        type            fixedValue;
        value           uniform 0;
    }
}

In this example, the inlet ﬁeld entry is read for the inlet patch, following rule 1 above (matching patch name). Similarly, the outletSmall entry will be read for the patch of the same name.

The outletMedium and outletLarge patches do not have matching entries in the ﬁeld ﬁle, so they instead the outlet entry will be applied (rule 2), since it matches the group name to which the patches belong. Note that the outletSmall patch does not use the outlet entry because a matching patch entry takes precedence over a matching group entry.

Finally, the lowerWall and upperWall match the regular expression ".*Wall". Regular expressions are described in section 4.2.13 ; they must be included in double quotations "…". The ".*" component matches any expression (including nothing), so matches the wall patch names here. The regular expression could use word grouping to provide a more precise match to the patch names, e.g.

    "(lower|upper)Wall"
    {
        type            zeroGradient;
    }

Alternatively a patch entry could cover the wall patches taking advantage of the fact that every non-generic patch is automatically placed in a group of the same name as its type, as discussed in section 5.3.6 . In this case, all wall patches are placed in a group named wall, so the following entry would be read for both patches.

    wall
    {
        type            zeroGradient;
    }

6.3.2 Geometric constraints

Section 5.3 describes the mesh boundary, which is split into patches and written in the mesh boundary ﬁle. Each patch includes a type entry which can be speciﬁed as a generic patch, a wall or a geometric constraint, e.g. empty, symmetry, cyclic etc.

For each geometric constraint type for a patch in the mesh, there is an equivalent boundary condition type that must be applied to the same patch in the boundaryField of a ﬁeld ﬁle. The type names in the mesh and boundaryField are the same, e.g. the symmetry boundary condition must be applied to a symmetry patch.

To simplify the conﬁguration of ﬁeld ﬁles, OpenFOAM includes a ﬁle named setConstraintTypes in the $FOAM_ETC/caseDicts of the installation. The setConstraintTypes ﬁle contains the following entries.

9cyclic

10{

11    type  cyclic;

12}

13

14cyclicSlip

15{

16    type  cyclicSlip;

17}

18

19nonConformalCyclic

20{

21    type  nonConformalCyclic;

22}

23

24nonConformalError

25{

26    type  nonConformalError;

27}

28

29empty

30{

31    type  empty;

32}

33

34processor

35{

36    type  processor;

37}

38

39processorCyclic

40{

41    type  processorCyclic;

42}

43

44nonConformalProcessorCyclic

45{

46    type  nonConformalProcessorCyclic;

47}

48

49symmetryPlane

50{

51    type  symmetryPlane;

52}

53

54symmetry

55{

56    type  symmetry;

57}

58

59wedge

60{

61    type  wedge;

62}

63

64internal

65{

66    type  internal;

67}

68

69

70// ************************************************************************* //

The ﬁle exploits the fact that a patch which is a geometric constraint is automatically included in a group of the constraint name, e.g. a symmetry patch is in a group named symmetry. The entries therefore set a boundary type for each constraint group (to the name of the group). All constraint conditions are covered by an entry for each condition.

The user can then include this ﬁle inside the boundaryField of their ﬁeld ﬁles. Since the ﬁle is in the $FOAM_ETC directory it can be included using the special #includeEtc directive, e.g. in the boundaryField entry below.

boundaryField
{
    inlet
    {
        type            zeroGradient;
    }

    outlet
    {
        type            fixedValue;
        value           uniform 0;
    }

    wall
    {
        type            zeroGradient;
    }

    #includeEtc "caseDicts/setConstraintTypes"
}

With the setContraintTypes ﬁle included in the ﬁeld ﬁles, the only patches that generally need to be conﬁgured are: the generic patches, corresponding to open boundaries; and, wall patches.

6.3.3 Basic boundary conditions

The main basic boundary condition types available in OpenFOAM are summarised below using a patch ﬁeld named $\text{[math]}$ . This is not a complete list; for all types see $FOAM_SRC/ﬁniteVolume/ﬁelds/fvPatchFields/basic.

ﬁxedValue : value of $\text{[math]}$ is speciﬁed by value .
ﬁxedGradient : normal gradient of $\text{[math]}$ ( $\text{[math]}$ ) is speciﬁed by gradient.
zeroGradient : normal gradient of $\text{[math]}$ is zero.
calculated : patch ﬁeld $\text{[math]}$ calculated from other patch ﬁelds.
mixed : mixed ﬁxedValue/ ﬁxedGradient condition depending on valueFraction $\text{[math]}$ where

${1 corresponds to Ψ = refValue, valueFraction = 0 corresponds to ∂Ψ ∕∂n = refGradient. \relax \special {t4ht=$ (6.2)
directionMixed : mixed condition with tensorial valueFraction , to allow diﬀerent conditions in normal and tangential directions of a vector patch ﬁeld, e.g. ﬁxedValue in the tangential direction, zeroGradient in the normal direction.

OpenFOAM v14 User Guide - 6.3 Introduction to boundary conditions

CFD Direct

OpenFOAM v14 User Guide - 6.3 Introduction to boundary conditions

How are boundary conditions applied in CFD?

6.3 Introduction to boundary conditions

6.3.1 Patch selection in ﬁeld ﬁles

6.3.2 Geometric constraints

6.3.3 Basic boundary conditions