ENH: freestream BC: allow inlet value to be specified by another patch

The freestreamFvPatchField previously employed a fixed value when supplying
the inlet values.  This commit extends the BC so that users can use another
patch to supply the values via the new freestreamBC entry, e.g. to set the
velocity to an atmospheric boundary layer profile:

    inlet
    {
        type            freestream;
        freestreamBC
        {
            type            atmBoundaryLayerInletVelocity;
            flowDir         (1 0 0);
            zDir            (0 0 1);
            Uref            20;
            Zref            20;
            z0              uniform 0.1;
            zGround         uniform 935;
        }
    }

The earlier specification is also maintained for backwards compatibility, e.g.

    inlet
    {
        type            freestream;
        freestreamValue uniform (300 0 0);
    }

src/finiteVolume/fields/fvPatchFields/derived/freestream/freestreamFvPatchField.C

@@ -3,7 +3,7 @@
   \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
    \\    /   O peration     |
     \\  /    A nd           | Copyright (C) 2011-2015 OpenFOAM Foundation
-     \\/     M anipulation  | Copyright (C) 2017 OpenCFD Ltd.
+     \\/     M anipulation  | Copyright (C) 2017-2018 OpenCFD Ltd.
 -------------------------------------------------------------------------------
 License
     This file is part of OpenFOAM.
@@ -34,7 +34,8 @@ Foam::freestreamFvPatchField<Type>::freestreamFvPatchField
     const DimensionedField<Type, volMesh>& iF
 )
 :
-    inletOutletFvPatchField<Type>(p, iF)
+    inletOutletFvPatchField<Type>(p, iF),
+    freestreamBCPtr_()
 {}
 
 
@@ -46,13 +47,17 @@ Foam::freestreamFvPatchField<Type>::freestreamFvPatchField
     const dictionary& dict
 )
 :
-    inletOutletFvPatchField<Type>(p, iF)
+    inletOutletFvPatchField<Type>(p, iF),
+    freestreamBCPtr_()
 {
     this->patchType() = dict.lookupOrDefault<word>("patchType", word::null);
 
     this->phiName_ = dict.lookupOrDefault<word>("phi","phi");
 
-    freestreamValue() = Field<Type>("freestreamValue", dict, p.size());
+    if (dict.found("freestreamValue"))
+    {
+        freestreamValue() =
+            Field<Type>("freestreamValue", dict, p.size());
 
         if (dict.found("value"))
         {
@@ -66,6 +71,20 @@ Foam::freestreamFvPatchField<Type>::freestreamFvPatchField
             fvPatchField<Type>::operator=(freestreamValue());
         }
     }
+    else
+    {
+        // Freestream value provided by another patch
+        freestreamBCPtr_ =
+            fvPatchField<Type>::New(p, iF, dict.subDict("freestreamBC"));
+
+        // Force user to supply an initial value
+        // - we do not know if the supplied BC has all dependencies available
+        fvPatchField<Type>::operator=
+        (
+            Field<Type>("value", dict, p.size())
+        );
+    }
+}
 
 
 template<class Type>
@@ -77,8 +96,15 @@ Foam::freestreamFvPatchField<Type>::freestreamFvPatchField
     const fvPatchFieldMapper& mapper
 )
 :
-    inletOutletFvPatchField<Type>(ptf, p, iF, mapper)
+    inletOutletFvPatchField<Type>(ptf, p, iF, mapper),
-{}
+    freestreamBCPtr_()
+{
+    if (ptf.freestreamBCPtr_.valid())
+    {
+        freestreamBCPtr_ =
+            fvPatchField<Type>::New(ptf.freestreamBCPtr_(), p, iF, mapper);
+    }
+}
 
 
 template<class Type>
@@ -87,8 +113,14 @@ Foam::freestreamFvPatchField<Type>::freestreamFvPatchField
     const freestreamFvPatchField<Type>& ptf
 )
 :
-    inletOutletFvPatchField<Type>(ptf)
+    inletOutletFvPatchField<Type>(ptf),
-{}
+    freestreamBCPtr_()
+{
+    if (ptf.freestreamBCPtr_.valid())
+    {
+        freestreamBCPtr_ = ptf.freestreamBCPtr_->clone();
+    }
+}
 
 
 template<class Type>
@@ -98,18 +130,81 @@ Foam::freestreamFvPatchField<Type>::freestreamFvPatchField
     const DimensionedField<Type, volMesh>& iF
 )
 :
-    inletOutletFvPatchField<Type>(ptf, iF)
+    inletOutletFvPatchField<Type>(ptf, iF),
-{}
+    freestreamBCPtr_()
+{
+    if (ptf.freestreamBCPtr_.valid())
+    {
+        freestreamBCPtr_ = ptf.freestreamBCPtr_->clone();
+    }
+}
 
 
 // * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
 
+template<class Type>
+void Foam::freestreamFvPatchField<Type>::autoMap(const fvPatchFieldMapper& m)
+{
+    inletOutletFvPatchField<Type>::autoMap(m);
+    if (freestreamBCPtr_.valid())
+    {
+        freestreamBCPtr_->autoMap(m);
+    }
+}
+
+
+template<class Type>
+void Foam::freestreamFvPatchField<Type>::rmap
+(
+    const fvPatchField<Type>& ptf,
+    const labelList& addr
+)
+{
+    inletOutletFvPatchField<Type>::rmap(ptf, addr);
+
+    const auto& fsptf = refCast<const freestreamFvPatchField<Type>>(ptf);
+
+    if (fsptf.freestreamBCPtr_.valid())
+    {
+        freestreamBCPtr_->rmap(fsptf.freestreamBCPtr_(), addr);
+    }
+}
+
+
+template<class Type>
+void Foam::freestreamFvPatchField<Type>::updateCoeffs()
+{
+    if (this->updated())
+    {
+        return;
+    }
+
+    if (freestreamBCPtr_.valid())
+    {
+        freestreamBCPtr_->evaluate();
+        freestreamValue() = freestreamBCPtr_();
+    }
+
+    inletOutletFvPatchField<Type>::updateCoeffs();
+}
+
+
 template<class Type>
 void Foam::freestreamFvPatchField<Type>::write(Ostream& os) const
 {
     fvPatchField<Type>::write(os);
     os.writeEntryIfDifferent<word>("phi", "phi", this->phiName_);
+
+    if (freestreamBCPtr_.valid())
+    {
+        os.beginBlock("freestreamBC");
+        freestreamBCPtr_->write(os);
+        os.endBlock();
+    }
+    else
+    {
         freestreamValue().writeEntry("freestreamValue", os);
+    }
     this->writeEntry("value", os);
 }
 

src/finiteVolume/fields/fvPatchFields/derived/freestream/freestreamFvPatchField.H

@@ -3,7 +3,7 @@
   \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
    \\    /   O peration     |
     \\  /    A nd           | Copyright (C) 2011-2018 OpenFOAM Foundation
-     \\/     M anipulation  |
+     \\/     M anipulation  | Copyright (C) 2018 OpenCFD Ltd.
 -------------------------------------------------------------------------------
 License
     This file is part of OpenFOAM.
@@ -36,11 +36,13 @@ Description
 Usage
     \table
         Property        | Description           | Required    | Default value
-        freestreamValue   | freestream velocity          | yes         |
+        freestreamValue | freestream velocity   | no          |
+        freestreamBC    | patchField providing the inlet field | no  |
         phi             | flux field name       | no          | phi
     \endtable
 
-    Example of the boundary condition specification:
+    Example of the boundary condition specification using a fixed value
+    inlet condition:
     \verbatim
     <patchName>
     {
@@ -49,6 +51,26 @@ Usage
     }
     \endverbatim
 
+    Example of the boundary condition specification using a separate condition
+    to proveide the inlet condition:
+    \verbatim
+    <patchName>
+    {
+        type            freestream;
+        freestreamBC
+        {
+            type            atmBoundaryLayerInletVelocity;
+            flowDir         (1 0 0);
+            zDir            (0 0 1);
+            Uref            20;
+            Zref            20;
+            z0              uniform 0.1;
+            zGround         uniform 935;
+        }
+    }
+    \endverbatim
+
+
 See also
     Foam::mixedFvPatchField
     Foam::inletOutletFvPatchField
@@ -77,6 +99,11 @@ class freestreamFvPatchField
 :
     public inletOutletFvPatchField<Type>
 {
+    // Private data
+
+        //- BC to supply the freestream value
+        tmp<fvPatchField<Type>> freestreamBCPtr_;
+
 
 public:
 
@@ -147,6 +174,22 @@ public:
 
     // Member functions
 
+        // Mapping functions
+
+            //- Map (and resize as needed) from self given a mapping object
+            virtual void autoMap(const fvPatchFieldMapper& mapper);
+
+            //- Reverse map the given fvPatchField onto this fvPatchField
+            virtual void rmap
+            (
+                const fvPatchField<Type>& ptf,
+                const labelList& addr
+            );
+
+
+        //- Update the coefficients associated with the patch field
+        virtual void updateCoeffs();
+
         // Return defining fields
 
             const Field<Type>& freestreamValue() const