surfaceInterpolate

Table of Contents

• Description
  • Operands
• Usage
• Further information

Description

The surfaceInterpolate function object linearly interpolates volume fields to generate surface fields.

Operands

Operand	Type	Location
input	vol<Type>Field	$FOAM_CASE/<time>/<inpField>
output file	-	-
output field	surface<Type>Field	$FOAM_CASE/<time>/<outField>

where <Type>=Scalar/Vector/SphericalTensor/SymmTensor/Tensor.

Usage

Example of the surfaceInterpolate function object by using functions sub-dictionary in system/controlDict file:

surfaceInterpolate1
{
    // Mandatory entries (unmodifiable)
    type            surfaceInterpolate;
    libs            (fieldFunctionObjects);

    // Mandatory entries (runtime modifiable)
    fields      ((<inpField1> <outField1>) ... (<inpFieldN> <outFieldN>));

    // Optional (inherited) entries
    region          region0;
    enabled         true;
    log             true;
    timeStart       0;
    timeEnd         1000;
    executeControl  timeStep;
    executeInterval 1;
    writeControl    timeStep;
    writeInterval   1;
}

where the entries mean:

Property	Description	Type	Required	Default
type	Type name: surfaceInterpolate	word	yes	-
libs	Library name: fieldFunctionObjects	word	yes	-
fields	Names of operand and output fields	wordList	yes	-

The inherited entries are elaborated in:

• functionObject

Usage by the postProcess utility is not available.

Further information

Tutorial:

• $FOAM_TUTORIALS/incompressible/pisoFoam/RAS/cavity

Source code:

• Foam::functionObjects::surfaceInterpolate

History

• Introduced in version v1606+