This boundary condition provides a waveVelocity condition. This sets the velocity to that specified by a superposition of wave models. The corresponding phase fraction and pressure conditions look this condition up and re-use the wave modelling. More...

Inheritance diagram for waveVelocityFvPatchVectorField:

[legend]

Collaboration diagram for waveVelocityFvPatchVectorField:

[legend]

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

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

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

	waveVelocityFvPatchVectorField (const waveVelocityFvPatchVectorField &, const fvPatch &, const DimensionedField< vector, volMesh > &, const fvPatchFieldMapper &)
	Construct by mapping given mixedTypeFvPatchField onto a new patch. More...

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

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

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

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

const word &	pName () const
	Access the name of the pressure field. More...

const waveSuperposition &	waves () const
	Access the wave models. More...

const fvMeshSubset &	faceCellSubset () const
	Access the face-cell subset. More...

tmp< vectorField >	U () const
	Return the current modelled velocity field on the patch faces. More...

tmp< vectorField >	Un () const
	Return the current modelled velocity field in the neighbour cell. More...

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

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

Detailed Description

This boundary condition provides a waveVelocity condition. This sets the velocity to that specified by a superposition of wave models. The corresponding phase fraction and pressure conditions look this condition up and re-use the wave modelling.

Flow reversal will occur in the event that the amplitude of the velocity oscillation is greater than the mean flow. This triggers special handling, the form of which depends on the inletOutlet flag and whether a wave pressure condition is being used.

If a wave pressure condition is not being used, and inletOutlet is false, then this is a standard fixed value condition, with the value supplied by the wave model. If flow reversal occurs this state may be unstable. The corresponding pressure condition should be fixedFluxPressure.

If a wave pressure condition is not being used, and inletOutlet is true or not specified then the proportion of the patch over which the flow is reversed functions in a manner similar to the flowRateOutletVelocity condition; i.e., the velocity is extrapolated and then scaled to match the required outlet flow rate. Numerically, this is still a fixedValue constraint on the normal velocity, just one which tends to avoid instability. Again, the corresponding pressure condition should be fixedFluxPressure.

If a wave pressure condition is being used, then the normal velocity condition becomes fixedGradient on outlet faces. This gradient is calculated numerically by evaluating the wave model on both the patch face and the adjacent cell. The pressure boundary in this case should be a wavePressure condition. This will do the opposite; it will fix the pressure value on outlet faces, and the gradient otherwise.

Usage

Property	Description	Req'd?	Default
`phi`	Name of the flux field	no	phi
`p`	Name of the pressure field	no	p
`inletOutlet`	does the condition behave like inletOutlet	no	true
`origin`	origin of the wave coordinate system	yes
`direction`	direction of the mean flow	yes
`speed`	speed of the mean flow	yes
`waves`	list of wave models to superimpose	yes
`ramp`	ramping function for the mean flow speed	no	None
`scale`	scale factor along the mean flow direction	no	None
`crossScale`	scale factor across the mean flow direction	no	None
`heightAboveWave`	use with the height above the wave	no	false

Example of the boundary condition specification:

    <patchName>
    {
        type        waveVelocity;
        origin      (0 25 0);
        direction   (1 0 0);
        speed       2;
        waves
        (
            Airy
            {
                length      40;
                amplitude   0.5;
                phase       0;
                angle       0;
            }
            Airy
            {
                length      20;
                amplitude   0.25;
                phase       1.5708;
                angle       0;
            }
        );
        ramp        constant 1;
        scale       table ((100 1) (200 0));
        crossScale  constant 1;
    }

Source files

Definition at line 187 of file waveVelocityFvPatchVectorField.H.

Constructor & Destructor Documentation

◆ waveVelocityFvPatchVectorField() [1/5]

waveVelocityFvPatchVectorField	(	const fvPatch &	p,
		const DimensionedField< vector, volMesh > &	iF
	)

Construct from patch and internal field.

Definition at line 36 of file waveVelocityFvPatchVectorField.C.

References Foam::Zero.

Referenced by waveVelocityFvPatchVectorField::clone(), and waveVelocityFvPatchVectorField::waveVelocityFvPatchVectorField().

Here is the caller graph for this function:

◆ waveVelocityFvPatchVectorField() [2/5]

waveVelocityFvPatchVectorField	(	const fvPatch &	p,
		const DimensionedField< vector, volMesh > &	iF,
		const dictionary &	dict
	)

Construct from patch, internal field and dictionary.

Definition at line 56 of file waveVelocityFvPatchVectorField.C.

References dictionary::found(), fvPatch::size(), vectorField(), waveVelocityFvPatchVectorField::waveVelocityFvPatchVectorField(), and Foam::Zero.

Here is the call graph for this function:

◆ waveVelocityFvPatchVectorField() [3/5]

waveVelocityFvPatchVectorField	(	const waveVelocityFvPatchVectorField &	ptf,
		const fvPatch &	p,
		const DimensionedField< vector, volMesh > &	iF,
		const fvPatchFieldMapper &	mapper
	)