totalPressureFvPatchScalarField, uniformTotalPressureFvPatchScalarField: simplified and rationalized

The modes of operation are set by the dimensions of the pressure field
    to which this boundary condition is applied, the \c psi entry and the value
    of \c gamma:
    \table
        Mode                    | dimensions | psi   | gamma
        incompressible subsonic | p/rho      |       |
        compressible subsonic   | p          | none  |
        compressible transonic  | p          | psi   | 1
        compressible supersonic | p          | psi   | > 1
    \endtable

    For most applications the totalPressure boundary condition now only
    requires p0 to be specified e.g.
    outlet
    {
        type            totalPressure;
        p0              uniform 1e5;
    }

src/finiteVolume/fields/fvPatchFields/derived/totalPressure/totalPressureFvPatchScalarField.C

@@ -41,7 +41,7 @@ Foam::totalPressureFvPatchScalarField::totalPressureFvPatchScalarField
     fixedValueFvPatchScalarField(p, iF),
     UName_("U"),
     phiName_("phi"),
-    rhoName_("none"),
+    rhoName_("rho"),
     psiName_("none"),
     gamma_(0.0),
     p0_(p.size(), 0.0)
@@ -58,9 +58,9 @@ Foam::totalPressureFvPatchScalarField::totalPressureFvPatchScalarField
     fixedValueFvPatchScalarField(p, iF),
     UName_(dict.lookupOrDefault<word>("U", "U")),
     phiName_(dict.lookupOrDefault<word>("phi", "phi")),
-    rhoName_(dict.lookupOrDefault<word>("rho", "none")),
+    rhoName_(dict.lookupOrDefault<word>("rho", "rho")),
     psiName_(dict.lookupOrDefault<word>("psi", "none")),
-    gamma_(readScalar(dict.lookup("gamma"))),
+    gamma_(psiName_ != "none" ? readScalar(dict.lookup("gamma")) : 1),
     p0_("p0", dict, p.size())
 {
     if (dict.found("value"))
@@ -167,18 +167,27 @@ void Foam::totalPressureFvPatchScalarField::updateCoeffs
     const fvsPatchField<scalar>& phip =
         patch().lookupPatchField<surfaceScalarField, scalar>(phiName_);
 
-    if (psiName_ == "none" && rhoName_ == "none")
+    if (internalField().dimensions() == dimPressure)
     {
-        operator==(p0p - 0.5*(1.0 - pos(phip))*magSqr(Up));
+        if (psiName_ == "none")
+        {
+            // Variable density and low-speed compressible flow
+
+            const fvPatchField<scalar>& rho =
+                patch().lookupPatchField<volScalarField, scalar>(rhoName_);
+
+            operator==(p0p - 0.5*rho*(1.0 - pos(phip))*magSqr(Up));
         }
-    else if (rhoName_ == "none")
+        else
         {
+            // High-speed compressible flow
+
             const fvPatchField<scalar>& psip =
                 patch().lookupPatchField<volScalarField, scalar>(psiName_);
 
-        if (gamma_ > 1.0)
+            if (gamma_ > 1)
             {
-            scalar gM1ByG = (gamma_ - 1.0)/gamma_;
+                scalar gM1ByG = (gamma_ - 1)/gamma_;
 
                 operator==
                 (
@@ -195,21 +204,22 @@ void Foam::totalPressureFvPatchScalarField::updateCoeffs
                 operator==(p0p/(1.0 + 0.5*psip*(1.0 - pos(phip))*magSqr(Up)));
             }
         }
-    else if (psiName_ == "none")
-    {
-        const fvPatchField<scalar>& rho =
-            patch().lookupPatchField<volScalarField, scalar>(rhoName_);
 
-        operator==(p0p - 0.5*rho*(1.0 - pos(phip))*magSqr(Up));
+    }
+    else if (internalField().dimensions() == dimPressure/dimDensity)
+    {
+        // Incompressible flow
+        operator==(p0p - 0.5*(1.0 - pos(phip))*magSqr(Up));
     }
     else
     {
         FatalErrorInFunction
-            << " rho or psi set inconsistently, rho = " << rhoName_
+            << " Incorrect pressure dimensions " << internalField().dimensions()
-            << ", psi = " << psiName_ << ".\n"
+            << nl
-            << "    Set either rho or psi or neither depending on the "
+            << "    Should be " << dimPressure
-               "definition of total pressure." << nl
+            << " for compressible/variable density flow" << nl
-            << "    Set the unused variable(s) to 'none'.\n"
+            << "    or " << dimPressure/dimDensity
+            << " for incompressible flow," << nl
             << "    on patch " << this->patch().name()
             << " of field " << this->internalField().name()
             << " in file " << this->internalField().objectPath()

src/finiteVolume/fields/fvPatchFields/derived/totalPressure/totalPressureFvPatchScalarField.H

@@ -54,7 +54,7 @@ Description
             U       | velocity
         \endvartable
 
-    3. compressible transonic (\f$\gamma <= 1\f$):
+    3. compressible transonic (\f$\gamma = 1\f$):
         \f[
             p_p = \frac{p_0}{1 + 0.5 \psi |U|^2}
         \f]
@@ -78,14 +78,15 @@ Description
             G       | coefficient given by \f$\frac{\gamma}{1-\gamma}\f$
         \endvartable
 
-    The modes of operation are set via the combination of \c phi, \c rho, and
+    The modes of operation are set by the dimensions of the pressure field
-    \c psi entries:
+    to which this boundary condition is applied, the \c psi entry and the value
+    of \c gamma:
     \table
-        Mode                    | phi   | rho   | psi
+        Mode                    | dimensions | psi   | gamma
-        incompressible subsonic | phi   | none  | none
+        incompressible subsonic | p/rho      |       |
-        compressible subsonic   | phi   | rho   | none
+        compressible subsonic   | p          | none  |
-        compressible transonic  | phi   | none  | psi
+        compressible transonic  | p          | psi   | 1
-        compressible supersonic | phi   | none  | psi
+        compressible supersonic | p          | psi   | > 1
     \endtable
 
 
@@ -93,12 +94,12 @@ Description
 
     \table
         Property     | Description                | Required | Default value
-        U            | velocity field name     | no          | U
+        U            | Velocity field name        | no       | U
-        phi          | flux field name         | no          | phi
+        phi          | Flux field name            | no       | phi
-        rho          | density field name      | no          | none
+        rho          | Density field name         | no       | rho
-        psi          | compressibility field name | no       | none
+        psi          | Compressibility field name | no       | none
-        gamma        | ratio of specific heats (Cp/Cv) | yes |
+        gamma        | (Cp/Cv)                    | no       | 1
-        p0           | total pressure          | yes       |
+        p0           | Total pressure             | yes      |
     \endtable
 
     Example of the boundary condition specification:
@@ -106,18 +107,10 @@ Description
     myPatch
     {
         type            totalPressure;
-        U               U;
-        phi             phi;
-        rho             none;
-        psi             none;
-        gamma           1.4;
         p0              uniform 1e5;
     }
     \endverbatim
 
-Note
-    The default boundary behaviour is for subsonic, incompressible flow.
-
 SeeAlso
     Foam::fixedValueFvPatchField
 

src/finiteVolume/fields/fvPatchFields/derived/uniformTotalPressure/uniformTotalPressureFvPatchScalarField.C

@@ -41,10 +41,10 @@ uniformTotalPressureFvPatchScalarField
     fixedValueFvPatchScalarField(p, iF),
     UName_("U"),
     phiName_("phi"),
-    rhoName_("none"),
+    rhoName_("rho"),
     psiName_("none"),
     gamma_(0.0),
-    pressure_()
+    p0_()
 {}
 
 
@@ -59,10 +59,10 @@ uniformTotalPressureFvPatchScalarField
     fixedValueFvPatchScalarField(p, iF),
     UName_(dict.lookupOrDefault<word>("U", "U")),
     phiName_(dict.lookupOrDefault<word>("phi", "phi")),
-    rhoName_(dict.lookupOrDefault<word>("rho", "none")),
+    rhoName_(dict.lookupOrDefault<word>("rho", "rho")),
     psiName_(dict.lookupOrDefault<word>("psi", "none")),
-    gamma_(readScalar(dict.lookup("gamma"))),
+    gamma_(psiName_ != "none" ? readScalar(dict.lookup("gamma")) : 1),
-    pressure_(Function1<scalar>::New("pressure", dict))
+    p0_(Function1<scalar>::New("p0", dict))
 {
     if (dict.found("value"))
     {
@@ -74,7 +74,7 @@ uniformTotalPressureFvPatchScalarField
     else
     {
         const scalar t = this->db().time().timeOutputValue();
-        fvPatchScalarField::operator==(pressure_->value(t));
+        fvPatchScalarField::operator==(p0_->value(t));
     }
 }
 
@@ -94,14 +94,14 @@ uniformTotalPressureFvPatchScalarField
     rhoName_(ptf.rhoName_),
     psiName_(ptf.psiName_),
     gamma_(ptf.gamma_),
-    pressure_(ptf.pressure_, false)
+    p0_(ptf.p0_, false)
 {
     patchType() = ptf.patchType();
 
     // Set the patch pressure to the current total pressure
     // This is not ideal but avoids problems with the creation of patch faces
     const scalar t = this->db().time().timeOutputValue();
-    fvPatchScalarField::operator==(pressure_->value(t));
+    fvPatchScalarField::operator==(p0_->value(t));
 }
 
 
@@ -117,7 +117,7 @@ uniformTotalPressureFvPatchScalarField
     rhoName_(ptf.rhoName_),
     psiName_(ptf.psiName_),
     gamma_(ptf.gamma_),
-    pressure_(ptf.pressure_, false)
+    p0_(ptf.p0_, false)
 {}
 
 
@@ -134,7 +134,7 @@ uniformTotalPressureFvPatchScalarField
     rhoName_(ptf.rhoName_),
     psiName_(ptf.psiName_),
     gamma_(ptf.gamma_),
-    pressure_(ptf.pressure_, false)
+    p0_(ptf.p0_, false)
 {}
 
 
@@ -150,23 +150,32 @@ void Foam::uniformTotalPressureFvPatchScalarField::updateCoeffs
         return;
     }
 
-    scalar p0 = pressure_->value(this->db().time().timeOutputValue());
+    scalar p0 = p0_->value(this->db().time().timeOutputValue());
 
     const fvsPatchField<scalar>& phip =
         patch().lookupPatchField<surfaceScalarField, scalar>(phiName_);
 
-    if (psiName_ == "none" && rhoName_ == "none")
+    if (internalField().dimensions() == dimPressure)
     {
-        operator==(p0 - 0.5*(1.0 - pos(phip))*magSqr(Up));
+        if (psiName_ == "none")
+        {
+            // Variable density and low-speed compressible flow
+
+            const fvPatchField<scalar>& rho =
+                patch().lookupPatchField<volScalarField, scalar>(rhoName_);
+
+            operator==(p0 - 0.5*rho*(1.0 - pos(phip))*magSqr(Up));
         }
-    else if (rhoName_ == "none")
+        else
         {
+            // High-speed compressible flow
+
             const fvPatchField<scalar>& psip =
                 patch().lookupPatchField<volScalarField, scalar>(psiName_);
 
-        if (gamma_ > 1.0)
+            if (gamma_ > 1)
             {
-            scalar gM1ByG = (gamma_ - 1.0)/gamma_;
+                scalar gM1ByG = (gamma_ - 1)/gamma_;
 
                 operator==
                 (
@@ -183,21 +192,22 @@ void Foam::uniformTotalPressureFvPatchScalarField::updateCoeffs
                 operator==(p0/(1.0 + 0.5*psip*(1.0 - pos(phip))*magSqr(Up)));
             }
         }
-    else if (psiName_ == "none")
-    {
-        const fvPatchField<scalar>& rho =
-            patch().lookupPatchField<volScalarField, scalar>(rhoName_);
 
-        operator==(p0 - 0.5*rho*(1.0 - pos(phip))*magSqr(Up));
+    }
+    else if (internalField().dimensions() == dimPressure/dimDensity)
+    {
+        // Incompressible flow
+        operator==(p0 - 0.5*(1.0 - pos(phip))*magSqr(Up));
     }
     else
     {
         FatalErrorInFunction
-            << " rho or psi set inconsitently, rho = " << rhoName_
+            << " Incorrect pressure dimensions " << internalField().dimensions()
-            << ", psi = " << psiName_ << ".\n"
+            << nl
-            << "    Set either rho or psi or neither depending on the "
+            << "    Should be " << dimPressure
-               "definition of total pressure.\n"
+            << " for compressible/variable density flow" << nl
-            << "    Set the unused variables to 'none'.\n"
+            << "    or " << dimPressure/dimDensity
+            << " for incompressible flow," << nl
             << "    on patch " << this->patch().name()
             << " of field " << this->internalField().name()
             << " in file " << this->internalField().objectPath()
@@ -222,7 +232,7 @@ void Foam::uniformTotalPressureFvPatchScalarField::write(Ostream& os) const
     os.writeKeyword("rho") << rhoName_ << token::END_STATEMENT << nl;
     os.writeKeyword("psi") << psiName_ << token::END_STATEMENT << nl;
     os.writeKeyword("gamma") << gamma_ << token::END_STATEMENT << nl;
-    pressure_->writeData(os);
+    p0_->writeData(os);
     writeEntry("value", os);
 }
 

src/finiteVolume/fields/fvPatchFields/derived/uniformTotalPressure/uniformTotalPressureFvPatchScalarField.H

@@ -29,18 +29,18 @@ Group
 
 Description
     This boundary condition provides a time-varying form of the uniform total
-    pressure boundary condition.
+    pressure boundary condition Foam::totalPressureFvPatchField.
 
     \heading Patch usage
 
     \table
         Property     | Description                | Required    | Default value
-        U            | velocity field name     | no          | U
+        U            | Velocity field name        | no          | U
-        phi          | flux field name         | no          | phi
+        phi          | Flux field name            | no          | phi
-        rho          | density field name      | no          | none
+        rho          | Density field name         | no          | rho
-        psi          | compressibility field name | no       | none
+        psi          | Compressibility field name | no          | none
-        gamma        | ratio of specific heats (Cp/Cv) | yes |
+        gamma        | (Cp/Cv)                    | no          | 1
-        pressure     | total pressure as a function of time | yes |
+        p0           | Total pressure as a function of time | yes |
     \endtable
 
     Example of the boundary condition specification:
@@ -48,22 +48,13 @@ Description
     myPatch
     {
         type            uniformTotalPressure;
-        U               U;
+        p0              uniform 1e5;
-        phi             phi;
-        rho             rho;
-        psi             psi;
-        gamma           1.4;
-        pressure        uniform 1e5;
     }
     \endverbatim
 
-    The \c pressure entry is specified as a Function1 type, able to describe
+    The \c p0 entry is specified as a Function1 type, able to describe
     time varying functions.
 
-Note
-    The default boundary behaviour is for subsonic, incompressible flow.
-
-
 SeeAlso
     Foam::Function1Types
     Foam::uniformFixedValueFvPatchField
@@ -112,7 +103,7 @@ class uniformTotalPressureFvPatchScalarField
         scalar gamma_;
 
         //- Table of time vs total pressure, including the bounding treatment
-        autoPtr<Function1<scalar>> pressure_;
+        autoPtr<Function1<scalar>> p0_;
 
 
 public:

tutorials/combustion/reactingFoam/laminar/counterFlowFlame2D/0/p

@@ -33,10 +33,6 @@ boundaryField
     {
         type            totalPressure;
         p0              $internalField;
-        rho             none;
-        psi             none;
-        gamma           1;
-        value           $internalField;
     }
     frontAndBack
     {

tutorials/combustion/reactingFoam/laminar/counterFlowFlame2DLTS/0/p

@@ -33,10 +33,6 @@ boundaryField
     {
         type            totalPressure;
         p0              $internalField;
-        rho             none;
-        psi             none;
-        gamma           1;
-        value           $internalField;
     }
     frontAndBack
     {

tutorials/compressible/rhoCentralDyMFoam/movingCone/0/p

@@ -39,10 +39,6 @@ boundaryField
     {
         type            totalPressure;
         p0              $internalField;
-        rho             none;
-        psi             none;
-        gamma           1;
-        value           $internalField;
     }
 
     farField

tutorials/compressible/rhoPimpleDyMFoam/annularThermalMixer/constant/boundaryConditions

@@ -42,11 +42,7 @@ outlet
     p
     {
         type            totalPressure;
-        value           uniform 1e5;
         p0              uniform 1e5;
-        rho             rho;
-        psi             none;
-        gamma           1.4;
     }
 
     U

tutorials/compressible/sonicDyMFoam/movingCone/0/p

@@ -39,10 +39,6 @@ boundaryField
     {
         type            totalPressure;
         p0              $internalField;
-        rho             none;
-        psi             none;
-        gamma           1;
-        value           $internalField;
     }
 
     farField

tutorials/incompressible/pimpleDyMFoam/movingCone/0/p

@@ -39,10 +39,6 @@ boundaryField
     {
         type            totalPressure;
         p0              $internalField;
-        rho             none;
-        psi             none;
-        gamma           1;
-        value           uniform 0;
     }
 
     farField

tutorials/incompressible/pimpleFoam/TJunction/0/p

@@ -23,16 +23,11 @@ boundaryField
     inlet
     {
         type            uniformTotalPressure;
-        pressure        table
+        p0              table
         (
             (0 10)
             (1 40)
         );
-        p0              40; // only used for restarts
-        rho             none;
-        psi             none;
-        gamma           1;
-        value           uniform 40;
     }
 
     outlet1

tutorials/incompressible/pimpleFoam/TJunctionFan/0.orig/p

@@ -24,17 +24,11 @@ boundaryField
     inlet
     {
         type            uniformTotalPressure;
-        rho             none;
+        p0              table
-        psi             none;
-        gamma           1;
-        pressure        table
-        2
         (
             (0 10)
             (1 40)
-        )
+        );
-        ;
-        value           uniform 40;
     }
     outlet1
     {

tutorials/lagrangian/reactingParcelFoam/counterFlowFlame2DLTS/0/p

@@ -33,10 +33,6 @@ boundaryField
     {
         type            totalPressure;
         p0              $internalField;
-        rho             none;
-        psi             none;
-        gamma           1;
-        value           $internalField;
     }
     frontAndBack
     {

tutorials/multiphase/cavitatingFoam/les/throttle/0/p

@@ -23,9 +23,6 @@ boundaryField
     inlet
     {
         type            totalPressure;
-        rho             rho;
-        psi             none;
-        gamma           1;
         p0              uniform 300e5;
     }
 

tutorials/multiphase/cavitatingFoam/les/throttle3D/0.orig/p

@@ -23,9 +23,6 @@ boundaryField
     inlet
     {
         type            totalPressure;
-        rho             rho;
-        psi             none;
-        gamma           1;
         p0              uniform 300e5;
     }
 

tutorials/multiphase/cavitatingFoam/ras/throttle/0/p

@@ -23,9 +23,6 @@ boundaryField
     inlet
     {
         type            totalPressure;
-        rho             rho;
-        psi             none;
-        gamma           1;
         p0              uniform 300e5;
     }
 

tutorials/multiphase/compressibleMultiphaseInterFoam/laminar/damBreak4phase/0.orig/p_rgh

@@ -42,10 +42,6 @@ boundaryField
     {
         type            totalPressure;
         p0              uniform 1e5;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           $internalField;
     }
 
     defaultFaces

tutorials/multiphase/interDyMFoam/ras/DTCHull/0.orig/p_rgh

@@ -39,10 +39,6 @@ boundaryField
     {
         type            totalPressure;
         p0              uniform 0;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           $internalField;
     }
 
     hull

tutorials/multiphase/interDyMFoam/ras/damBreakWithObstacle/0.orig/p_rgh

@@ -38,10 +38,6 @@ boundaryField
     {
         type            totalPressure;
         p0              uniform 0;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           uniform 0;
     }
 }
 

tutorials/multiphase/interDyMFoam/ras/floatingObject/0.orig/p_rgh

@@ -28,10 +28,6 @@ boundaryField
     {
         type            totalPressure;
         p0              uniform 0;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           uniform 0;
     }
     floatingObject
     {

tutorials/multiphase/interFoam/laminar/damBreak/damBreak/0/p_rgh

@@ -42,10 +42,6 @@ boundaryField
     {
         type            totalPressure;
         p0              uniform 0;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           uniform 0;
     }
 
     defaultFaces

tutorials/multiphase/interFoam/les/nozzleFlow2D/0/p_rgh

@@ -39,10 +39,6 @@ boundaryField
     {
         type            totalPressure;
         p0              uniform 0;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           uniform 0;
     }
 
     front

tutorials/multiphase/interFoam/ras/DTCHull/0.orig/p_rgh

@@ -39,10 +39,6 @@ boundaryField
     {
         type            totalPressure;
         p0              uniform 0;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           $internalField;
     }
 
     hull

tutorials/multiphase/interFoam/ras/damBreak/damBreak/0/p_rgh

@@ -42,10 +42,6 @@ boundaryField
     {
         type            totalPressure;
         p0              uniform 0;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           uniform 0;
     }
 
     defaultFaces

tutorials/multiphase/interFoam/ras/damBreakPorousBaffle/0/p_rgh

@@ -42,11 +42,7 @@ boundaryField
     atmosphere
     {
         type            totalPressure;
-        rho             rho;
-        psi             none;
-        gamma           1;
         p0              uniform 0;
-        value           uniform 0;
     }
     defaultFaces
     {

tutorials/multiphase/interFoam/ras/waterChannel/0/p_rgh

@@ -24,10 +24,6 @@ boundaryField
     {
         type            totalPressure;
         p0              uniform 0;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           uniform 0;
     }
 
     ".*"

tutorials/multiphase/interFoam/ras/weirOverflow/0.orig/p_rgh

@@ -41,10 +41,6 @@ boundaryField
     {
         type            totalPressure;
         p0              uniform 0;
-        rho             none;
-        psi             none;
-        gamma           1;
-        value           uniform $pressure;
     }
 
     defaultFaces

tutorials/multiphase/interMixingFoam/laminar/damBreak/0/p_rgh

@@ -42,10 +42,6 @@ boundaryField
     {
         type            totalPressure;
         p0              uniform 0;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           uniform 0;
     }
 
     defaultFaces

tutorials/multiphase/interPhaseChangeDyMFoam/propeller/0.orig/p_rgh

@@ -33,10 +33,6 @@ boundaryField
     {
         type            totalPressure;
         p0              $internalField;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           $internalField;
     }
 
     wall

tutorials/multiphase/multiphaseEulerFoam/damBreak4phase/0.orig/p_rgh

@@ -44,10 +44,6 @@ boundaryField
         p0              uniform 0;
         U               U.air;
         phi             phi.air;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           uniform 0;
     }
 
     defaultFaces

tutorials/multiphase/multiphaseEulerFoam/damBreak4phaseFine/0.orig/p_rgh

@@ -42,10 +42,6 @@ boundaryField
     {
         type            totalPressure;
         p0              uniform 0;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           uniform 0;
     }
 
     defaultFaces

tutorials/multiphase/multiphaseInterFoam/laminar/damBreak4phase/0.orig/p_rgh

@@ -42,10 +42,6 @@ boundaryField
     {
         type            totalPressure;
         p0              uniform 0;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           uniform 0;
     }
 
     defaultFaces

tutorials/multiphase/multiphaseInterFoam/laminar/damBreak4phaseFine/0.orig/p_rgh

@@ -42,10 +42,6 @@ boundaryField
     {
         type            totalPressure;
         p0              uniform 0;
-        rho             rho;
-        psi             none;
-        gamma           1;
-        value           uniform 0;
     }
 
     defaultFaces