This boundary condition tries to generate an inlet velocity that maintains a specified pressure drop between two face zones downstream. The zones should fully span a duct through which all the inlet flow passes. More...

Inheritance diagram for pressurePIDControlInletVelocityFvPatchVectorField:

[legend]

Collaboration diagram for pressurePIDControlInletVelocityFvPatchVectorField:

[legend]

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

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

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

	pressurePIDControlInletVelocityFvPatchVectorField (const pressurePIDControlInletVelocityFvPatchVectorField &, const fvPatch &, const DimensionedField< vector, volMesh > &, const fvPatchFieldMapper &)
	Construct by mapping given. More...

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

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

	pressurePIDControlInletVelocityFvPatchVectorField (const pressurePIDControlInletVelocityFvPatchVectorField &, 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...

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

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

Detailed Description

This boundary condition tries to generate an inlet velocity that maintains a specified pressure drop between two face zones downstream. The zones should fully span a duct through which all the inlet flow passes.

An incompressible, lossless analysis of the flow between the inlet and the two face-zones is performed. An ideal inlet velocity is thereby calculated from the user-specified pressure drop. This analysis can include the transient effect of the inlet velocity change. In this case, a shape factor is included to represent non-linearity in the duct cross section.

The average pressure drop between the two face zones is measured. The same incompressible, lossless analysis is performed using this pressure drop. The difference between the two computed velocities is considered as an error. The ideal inlet is modified so as to drive this error to zero. This is accomplished by means of a PID control algorithm, for which non-dimensional gains are specified by the user.

The shape factor takes a value of 0 for a linear change in cross sectional area between the two face zones. A value of 1 represents a step change in area at the mid-point between the zones. A smooth cubic or cosine profile between two zones with zero divergence is typically represented by a factor of between 0.2 and 0.25.

Patch usage

Property	Description	Required	Default value
`upstream`	upstream face zone name	yes
`downstream`	downstream face zone name	yes
`deltaP`	desired pressure drop	yes
`shapeFactor`	non-linearity in the nozzle	no	0
`p`	pressure field name	no	p
`phi`	flux field name	yes	phi
`rho`	density field name	no	none
`P`	proportional gain	yes
`I`	integral gain	yes
`D`	differential gain	yes

Example of the boundary condition specification:

    myPatch
    {
        type            pressurePIDControlInletVelocity;
        upstream        upstream;
        downstream      downstream;
        deltaP          200;
        shapeFactor     0;
        p               p;
        phi             phi;
        rho             none;
        P               0.5;
        I               0.5;
        D               0.1;
        value           uniform (0 0 0);
    }

See also: Foam::fixedValueFvPatchField

Source files

Definition at line 168 of file pressurePIDControlInletVelocityFvPatchVectorField.H.

Constructor & Destructor Documentation

◆ pressurePIDControlInletVelocityFvPatchVectorField() [1/5]

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

Construct from patch and internal field.

Definition at line 67 of file pressurePIDControlInletVelocityFvPatchVectorField.C.

◆ pressurePIDControlInletVelocityFvPatchVectorField() [2/5]

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

Construct from patch, internal field and dictionary.

Definition at line 125 of file pressurePIDControlInletVelocityFvPatchVectorField.C.

◆ pressurePIDControlInletVelocityFvPatchVectorField() [3/5]

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

Construct by mapping given.

flowRateInletVelocityFvPatchVectorField onto a new patch

Definition at line 95 of file pressurePIDControlInletVelocityFvPatchVectorField.C.

◆ pressurePIDControlInletVelocityFvPatchVectorField() [4/5]

pressurePIDControlInletVelocityFvPatchVectorField ( const pressurePIDControlInletVelocityFvPatchVectorField & ptf )

Construct as copy.

Definition at line 154 of file pressurePIDControlInletVelocityFvPatchVectorField.C.

◆ pressurePIDControlInletVelocityFvPatchVectorField() [5/5]

pressurePIDControlInletVelocityFvPatchVectorField	(	const pressurePIDControlInletVelocityFvPatchVectorField &	ptf,
		const DimensionedField< vector, volMesh > &	iF
	)