pressurePIDControlInletVelocity

Description

The pressurePIDControlInletVelocity is a velocity boundary condition that 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.

Usage

The condition requires entries in both the boundary and field files.

Boundary file

<patchName>
{
    type            patch;
    ...
}

Field file

<patchName>
{
    // Mandatory entries
    type                pressurePIDControlInletVelocity;
    upstream            <word>;
    downstream          <word>;
    deltaP              <scalar>;
    P                   <scalar>;
    I                   <scalar>;
    D                   <scalar>;

    // Optional entries
    shapeFactor         <scalar>;
    p                   <word>;
    phi                 <word>;
    rho                 <word>;
    error               <scalar>;
    errorIntegral       <scalar>;

    // Inherited entries
    ...
}

where:

Property	Description	Type	Required	Default
type	Type name: pressurePIDControlInletVelocity	word	yes	-
upstream	Name of the upstream face zone	word	yes	-
downstream	Name of the downstream face zone	word	yes	-
deltaP	Desired pressure difference between upstream and downstream	scalar	yes	-
P	Proportional gain	scalar	yes	-
I	Integral gain	scalar	yes	-
D	Derivative gain	scalar	yes	-
shapeFactor	Nozzle shape factor	scalar	no	0.0
phi	Name of flux field	word	no	phi
rho	Name of density field	word	no	rho
error	Error	scalar	no	0.0
errorIntegral	Error integral wrt time	scalar	no	0.0

The inherited entries are elaborated in:

• Foam::fixedValueFvPatchField

Further information

Tutorial:

• N/A

Source code:

• pressurePIDControlInletVelocity

API:

• Foam::pressurePIDControlInletVelocityFvPatchVectorField

History: Introduced in version v3.0+