OpenFOAM v14 User Guide - 6.5 Field functions in boundary conditions

6.5 Field functions in boundary conditions

Field functions are described in section 6.1 , where their use is demonstrated in initialising non-uniform internalFields within field files in a time directory, and in initialising fields within an fvModel configuration. Field functions can also be used to set non-uniform fields on boundary patches, i.e. to set different values on different faces of a patch. Field functions are used in boundary conditions firstly through the functionalFixedValue boundary condition which uses a field function to specify a non-uniform fixed value across a patch, see section 6.5.1 . They are specify particular parameters in a small number of boundary conditions described in section 6.5.2 and 6.6 .

6.5.1 The functionalFixedValue boundary condition

The functionalFixedValue boundary condition accompanies field functions, described in section 6.1 . Field functions allow the user to initialise non-uniform fields. While they are typically applied to the internalField, functionalFixedValue is a fixed value boundary condition where the values are specified with a field function.

The coded field function from section 6.1.3 provides a good example to illustrate the functionalFixedValue condition. Recall that the example initialises swirl flow according to Equation 6.1 , by the following configuration in the 0/U file.

The case specifically requires the same velocity distribution at the inlet patch. The functionalFixedValue enables this, with a value entry that is a field function. Since internalField is the same field function, the value entry can be specified using a macro expansion of internalField as follows. This will initialise the boundary condition according to the function specified above in the “evaluate #{…#};” block. The boundary values can also vary in time by specifying a function in an optional “update #{…#};” block. Recall that field functions include a reference named ‘t’ to the current time, which can be incorporated into a coded field function to make it a direct function of time.

6.5.2 Parameters as field functions

A small number of general boundary conditions have parameters which are implemented as field functions. The following foamFind command locates them.

One of the conditions is the pressureInletOutletVelocity condition, discussed in section 6.4.2 , where the tangentialVelocity parameter is a field function. Another is the freeStream condition where the freeStreamVelocity is a field function. The latter is used in the $FOAM_TUTORIALS/fluid/stackPlume example case to initialise the freeStreamVelocity in the far field with the atmosphericBoundaryLayerVelocity field function.