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

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:

Source code:

Foam::functionObjects::subtract

History

Introduced in version v1612+

Table of Contents

Description

Operands

Usage

Stored properties

Further information