This boundary condition provides a wall function for the turbulent viscosity (i.e. nut) based on velocity (i.e. U) using a binomial-function wall-function blending method between the viscous and inertial sublayer predictions of nut for low- and high-Reynolds number applications. More...

Inheritance diagram for nutUBlendedWallFunctionFvPatchScalarField:

[legend]

Collaboration diagram for nutUBlendedWallFunctionFvPatchScalarField:

[legend]

Public Member Functions
	TypeName ("nutUBlendedWallFunction")
	Runtime type information. More...

	nutUBlendedWallFunctionFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, volMesh > &)
	Construct from patch and internal field. More...

	nutUBlendedWallFunctionFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, volMesh > &, const dictionary &)
	Construct from patch, internal field and dictionary. More...

	nutUBlendedWallFunctionFvPatchScalarField (const nutUBlendedWallFunctionFvPatchScalarField &, const fvPatch &, const DimensionedField< scalar, volMesh > &, const fvPatchFieldMapper &)

	nutUBlendedWallFunctionFvPatchScalarField (const nutUBlendedWallFunctionFvPatchScalarField &)
	Construct as copy. More...

virtual tmp< fvPatchScalarField >	clone () const
	Construct and return a clone. More...

	nutUBlendedWallFunctionFvPatchScalarField (const nutUBlendedWallFunctionFvPatchScalarField &, const DimensionedField< scalar, volMesh > &)
	Construct as copy setting internal field reference. More...

virtual tmp< fvPatchScalarField >	clone (const DimensionedField< scalar, volMesh > &iF) const
	Construct and return a clone setting internal field reference. More...

virtual tmp< scalarField >	yPlus () const
	Calculate and return the yPlus at the boundary. More...

virtual void	write (Ostream &os) const
	Write. More...

Public Member Functions inherited from nutWallFunctionFvPatchScalarField
	TypeName ("nutWallFunction")
	Runtime type information. More...

	nutWallFunctionFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, volMesh > &)
	Construct from patch and internal field. More...

	nutWallFunctionFvPatchScalarField (const fvPatch &, const DimensionedField< scalar, volMesh > &, const dictionary &)
	Construct from patch, internal field and dictionary. More...

	nutWallFunctionFvPatchScalarField (const nutWallFunctionFvPatchScalarField &, const fvPatch &, const DimensionedField< scalar, volMesh > &, const fvPatchFieldMapper &)

	nutWallFunctionFvPatchScalarField (const nutWallFunctionFvPatchScalarField &)
	Construct as copy. More...

	nutWallFunctionFvPatchScalarField (const nutWallFunctionFvPatchScalarField &, const DimensionedField< scalar, volMesh > &)
	Construct as copy setting internal field reference. More...

virtual tmp< scalarField >	yPlus () const =0
	Calculate and return the yPlus at the boundary. More...

const wallFunctionCoefficients &	wallCoeffs () const noexcept
	Return wallFunctionCoefficients. More...

virtual void	updateCoeffs ()
	Update the coefficients associated with the patch field. More...

virtual void	write (Ostream &) const
	Write. More...

Protected Member Functions
virtual tmp< scalarField >	calcNut () const
	Calculate the turbulent viscosity. More...

tmp< scalarField >	calcUTau (const scalarField &magGradU) const
	Calculate the friction velocity. More...

void	writeLocalEntries (Ostream &) const
	Write local wall function variables. More...

Protected Member Functions inherited from nutWallFunctionFvPatchScalarField
virtual const volVectorField &	U (const turbulenceModel &turb) const

virtual void	checkType ()
	Check the type of the patch. More...

virtual tmp< scalarField >	calcNut () const =0
	Calculate the turbulent viscosity. More...

void	writeLocalEntries (Ostream &) const
	Write local wall function variables. More...

Protected Attributes
scalar	n_
	Model coefficient; default = 4. More...

Protected Attributes inherited from nutWallFunctionFvPatchScalarField
word	UName_
	Name of velocity field. More...

wallFunctionCoefficients	wallCoeffs_
	Wall-function coefficients. More...

Additional Inherited Members
Static Public Member Functions inherited from nutWallFunctionFvPatchScalarField
static const nutWallFunctionFvPatchScalarField &	nutw (const turbulenceModel &turbModel, const label patchi)
	Return the nut patchField for the given wall patch. More...

Detailed Description

This boundary condition provides a wall function for the turbulent viscosity (i.e. nut) based on velocity (i.e. U) using a binomial-function wall-function blending method between the viscous and inertial sublayer predictions of nut for low- and high-Reynolds number applications.

\[ u_\tau = (u_{\tau,vis}^n + u_{\tau,log}^n)^{1/n} \]

where

\( u_\tau \)	=	Friction velocity
\( u_{\tau,vis} \)	=	Friction velocity in the viscous sublayer
\( u_{\tau,log} \)	=	Friction velocity in the inertial sublayer

Reference:

        See the section that describes 'automatic wall treatment':
            Menter, F., Ferreira, J. C., Esch, T., Konno, B. (2003).
            The SST turbulence model with improved wall treatment
            for heat transfer predictions in gas turbines.
            In Proceedings of the International Gas Turbine Congress.
            November, 2003. Tokyo, Japan. pp. 2-7.

Usage

Example of the boundary condition specification:

<patchName>
{
    // Mandatory entries
    type            nutUBlendedWallFunction;

    // Optional entries
    n               4.0;

    // Inherited entries
    ...
 }

where the entries mean:

Property	Description	Type	Reqd	Deflt
`type`	Type name: nutUBlendedWallFunction	word	yes	-
`n`	Blending factor	scalar	no	4.0

The inherited entries are elaborated in:

nutWallFunctionFvPatchScalarField.H

Note

The full 'automatic wall treatment' description also requires use of the omegaWallFunctionFvPatchScalarField.H with the blending option binomial or with the deprecated blended flag set to on.
Suffers from non-exact restart since correctNut() (called through turbulence->validate) returns a slightly different value every time it is called. See nutUSpaldingWallFunctionFvPatchScalarField.C.

Source files

Definition at line 143 of file nutUBlendedWallFunctionFvPatchScalarField.H.

Constructor & Destructor Documentation

◆ nutUBlendedWallFunctionFvPatchScalarField() [1/5]

nutUBlendedWallFunctionFvPatchScalarField	(	const fvPatch &	p,
		const DimensionedField< scalar, volMesh > &	iF
	)

Construct from patch and internal field.

Definition at line 138 of file nutUBlendedWallFunctionFvPatchScalarField.C.

◆ nutUBlendedWallFunctionFvPatchScalarField() [2/5]

nutUBlendedWallFunctionFvPatchScalarField	(	const fvPatch &	p,
		const DimensionedField< scalar, volMesh > &	iF,
		const dictionary &	dict
	)

Construct from patch, internal field and dictionary.

Definition at line 164 of file nutUBlendedWallFunctionFvPatchScalarField.C.

◆ nutUBlendedWallFunctionFvPatchScalarField() [3/5]

nutUBlendedWallFunctionFvPatchScalarField	(	const nutUBlendedWallFunctionFvPatchScalarField &	ptf,
		const fvPatch &	p,
		const DimensionedField< scalar, volMesh > &	iF,
		const fvPatchFieldMapper &	mapper
	)

Construct by mapping given nutUBlendedWallFunctionFvPatchScalarField onto a new patch

Definition at line 150 of file nutUBlendedWallFunctionFvPatchScalarField.C.

◆ nutUBlendedWallFunctionFvPatchScalarField() [4/5]

nutUBlendedWallFunctionFvPatchScalarField ( const nutUBlendedWallFunctionFvPatchScalarField & wfpsf )

Construct as copy.

Definition at line 177 of file nutUBlendedWallFunctionFvPatchScalarField.C.

◆ nutUBlendedWallFunctionFvPatchScalarField() [5/5]

nutUBlendedWallFunctionFvPatchScalarField	(	const nutUBlendedWallFunctionFvPatchScalarField &	wfpsf,
		const DimensionedField< scalar, volMesh > &	iF
	)

Construct as copy setting internal field reference.

Definition at line 188 of file nutUBlendedWallFunctionFvPatchScalarField.C.

Member Function Documentation

◆ calcNut()

Foam::tmp< Foam::scalarField > calcNut ( ) const

protectedvirtual

Calculate the turbulent viscosity.

Implements nutWallFunctionFvPatchScalarField.

Definition at line 37 of file nutUBlendedWallFunctionFvPatchScalarField.C.

References nutUBlendedWallFunctionFvPatchScalarField::calcUTau(), IOobject::groupName(), Foam::mag(), Foam::max(), turbulenceModel::propertiesName, Foam::sqr(), and U.

Here is the call graph for this function:

◆ calcUTau()

Foam::tmp< Foam::scalarField > calcUTau ( const scalarField & magGradU ) const

protected

Calculate the friction velocity.

Definition at line 65 of file nutUBlendedWallFunctionFvPatchScalarField.C.

References e, forAll, IOobject::groupName(), Foam::log(), Foam::mag(), magUp, Foam::max(), n, Time::New(), fvPatchField< Type >::patchInternalField(), Foam::pow(), turbulenceModel::propertiesName, Foam::sqrt(), U, y, yPlus, and Foam::Zero.

Referenced by nutUBlendedWallFunctionFvPatchScalarField::calcNut().

Here is the call graph for this function:

Here is the caller graph for this function:

◆ writeLocalEntries()

void writeLocalEntries ( Ostream & os ) const

protected

Write local wall function variables.

Definition at line 127 of file nutUBlendedWallFunctionFvPatchScalarField.C.

References os(), and Ostream::writeEntryIfDifferent().

Here is the call graph for this function:

◆ TypeName()

TypeName ( "nutUBlendedWallFunction" )

Runtime type information.

◆ clone() [1/2]

virtual tmp< fvPatchScalarField > clone ( ) const

inlinevirtual

Construct and return a clone.

Definition at line 208 of file nutUBlendedWallFunctionFvPatchScalarField.H.

◆ clone() [2/2]

virtual tmp< fvPatchScalarField > clone ( const DimensionedField< scalar, volMesh > & iF ) const

inlinevirtual

Construct and return a clone setting internal field reference.

Definition at line 224 of file nutUBlendedWallFunctionFvPatchScalarField.H.

◆ yPlus()

Foam::tmp< Foam::scalarField > yPlus ( ) const

virtual

Calculate and return the yPlus at the boundary.

Implements nutWallFunctionFvPatchScalarField.

Definition at line 203 of file nutUBlendedWallFunctionFvPatchScalarField.C.

References IOobject::groupName(), Foam::mag(), turbulenceModel::propertiesName, fvPatchField< Type >::snGrad(), U, and y.

Here is the call graph for this function:

◆ write()

void write ( Ostream & os ) const

virtual

Write.

Reimplemented from nutWallFunctionFvPatchScalarField.

Definition at line 228 of file nutUBlendedWallFunctionFvPatchScalarField.C.

References os(), and ObukhovLength::write().

Here is the call graph for this function:

Member Data Documentation

◆ n_

scalar n_

protected

Model coefficient; default = 4.

Definition at line 152 of file nutUBlendedWallFunctionFvPatchScalarField.H.

The documentation for this class was generated from the following files:

src/TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUBlendedWallFunction/nutUBlendedWallFunctionFvPatchScalarField.H
src/TurbulenceModels/turbulenceModels/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUBlendedWallFunction/nutUBlendedWallFunctionFvPatchScalarField.C

Public Member Functions

Protected Member Functions

Protected Attributes

Additional Inherited Members

Detailed Description

Constructor & Destructor Documentation

◆ nutUBlendedWallFunctionFvPatchScalarField() [1/5]

◆ nutUBlendedWallFunctionFvPatchScalarField() [2/5]

◆ nutUBlendedWallFunctionFvPatchScalarField() [3/5]

◆ nutUBlendedWallFunctionFvPatchScalarField() [4/5]

◆ nutUBlendedWallFunctionFvPatchScalarField() [5/5]

Member Function Documentation

◆ calcNut()

◆ calcUTau()

◆ writeLocalEntries()

◆ TypeName()

◆ clone() [1/2]

◆ clone() [2/2]

◆ yPlus()

◆ write()

Member Data Documentation

◆ n_