Description🔗
The subtract
function object
subtracts a given list of (at least one or more)
fields from a field and produces a new field, where the fields possess the
same sizes and dimensions:
fieldResult = field1 - field2 - ... - fieldN
Operands🔗
Operand | Type | Location |
---|---|---|
input | {vol,surface}<Type>Field(s) |
$FOAM_CASE/<time>/<inpField>s |
output file | - | - |
output field | {vol,surface}<Type>Field |
$FOAM_CASE/<time>/<outField> |
where <Type>=Scalar/Vector/SphericalTensor/SymmTensor/Tensor
.
Usage🔗
Example of the add
function object
by using functions
sub-dictionary in system/controlDict
file:
subtract1
{
// Mandatory entries (unmodifiable)
type subtract;
libs (fieldFunctionObjects);
// Mandatory (inherited) entry (runtime modifiable)
fields (<field1> <field2> ... <fieldN>);
// Optional (inherited) entries
result <fieldResult>;
region region0;
subRegion region0;
enabled true;
log true;
timeStart 0;
timeEnd 1000;
executeControl timeStep;
executeInterval 1;
writeControl timeStep;
writeInterval 1;
}
The minimal set of entries comprise:
Property | Description | Type | Required | Default |
---|---|---|---|---|
type | Type name: subtract | word | yes | - |
libs | Library name: fieldFunctionObjects | word | yes | - |
field | Names of the operand fields | wordList | yes | - |
The inherited entries are elaborated in:
Example by using the postProcess
utility:
postProcess -func "subtract(<field1>, <field2>, ..., <fieldN>)"
Stored properties🔗
Fields🔗
The subtract
function object is stored on the mesh database,
using the default name:
subtract(<field1>,<field2>,...,<fieldN>)
This can be overridden by using the result
entry.
Further information🔗
Tutorial:
- $FOAM_TUTORIALS/multiphase/twoPhaseEulerFoam/laminar/bubbleColumn
- $FOAM_TUTORIALS/incompressible/pisoFoam/RAS/cavity
Source code:
API:
History:
- Introduced in version v1612+