OpenFOAM includes a collection of FunctionObjects that offer users the opportunity to closely manage their computational analyses. These objects can be applied to manipulate the workflow process, and provide a mechanism to extract predicted field and derived quantities at run-time. Alternatively, the actions can be executed afterwards using the execFlowFunctionObjects
utility.
The current range of features comprises of:
Function objects are defined by additional entries in the $FOAM_CASE/system/controlDict input dictionary. Each object is listed in a functions
sub-dictionary entry, e.g. the following shows the input options applicable to `output' -type objects:
functions { myFunctionObject // user-defined name of function object entry { type functionObjectType; libs (myFunctionObjectLib); region defaultRegion; enabled yes; timeStart 0; timeEnd 10; evaluateControl timeStep; evaluateInterval 1; writeControl writeTime; writeInterval 1; ... } }
Where:
Property | Description | Required | Default value |
---|---|---|---|
type | type of function object | yes | |
libs | libraries containing object implementation | yes | |
region | name of region for multi-region cases | no | |
enabled | on/off switch | no | yes |
timeStart | start time | no | |
timeEnd | end time | no | |
evaluateControl | when to evaluate: either 'writeTime' or 'timeStep' | no | timeStep |
evaluateInterval | steps between evaluation when evaluateControl=timeStep | no | 1 |
writeControl | when to output: either 'writeTime' or 'timeStep' | no | timeStep |
writeInterval | steps between output when writeControl=timeStep | no | 1 |
The sub-dictionary name myFunctionObject
is chosen by the user, and is typically used as the name of the output directory for any derived data. The type
entry defines the type of function object properties that follow. Since the function objects are packaged into separate libraries, the user must tell the code where to find the function object implementation, identified using the libs
entry.