fluentFvMesh.C

Go to the documentation of this file.

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | www.openfoam.com
     \\/     M anipulation  |
-------------------------------------------------------------------------------
    Copyright (C) 2011-2016 OpenFOAM Foundation
    Copyright (C) 2020-2023 OpenCFD Ltd.
-------------------------------------------------------------------------------
License
    This file is part of OpenFOAM.

    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.

    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.

    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.

\*---------------------------------------------------------------------------*/

#include <fstream>
#include <iostream>

using std::ios;

#include "Time.H"
#include "fluentFvMesh.H"
#include "primitiveMesh.H"
#include "wallFvPatch.H"
#include "symmetryPlaneFvPatch.H"
#include "symmetryFvPatch.H"
#include "cellModel.H"

// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //

Foam::fluentFvMesh::fluentFvMesh(const IOobject& io)
:
    fvMesh(io)
{}


// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //

void Foam::fluentFvMesh::writeFluentMesh() const
{
    // Make a directory called fluentInterface in the case
    mkDir(time().rootPath()/time().caseName()/"fluentInterface");

    // Open a file for the mesh
    std::ofstream fluentMeshFile
    (
        time().rootPath()
      / time().caseName()
      / "fluentInterface"
      / time().caseName() + ".msh"
    );

    Info<< "Writing Fluent Mesh" << endl;

    fluentMeshFile
        << "(0 \"OpenFOAM to Fluent Mesh File\")" << nl << nl
        << "(0 \"Dimension:\")" << nl
        << "(2 3)" << nl << nl
        << "(0 \"Grid dimensions:\")" << nl;

    // Writing number of points
    fluentMeshFile
            << "(10 (0 1 ";

    // Writing hex
    fluentMeshFile.setf(ios::hex, ios::basefield);

    fluentMeshFile
        << nPoints() << " 0 3))" << std::endl;

    // Writing number of cells
    fluentMeshFile
        << "(12 (0 1 "
        << nCells() << " 0 0))" << std::endl;

    // Writing number of faces
    label nFcs = nFaces();

    fluentMeshFile
            << "(13 (0 1 ";

    // Still writing hex
    fluentMeshFile
        << nFcs << " 0 0))" << std::endl << std::endl;

    // Return to dec
    fluentMeshFile.setf(ios::dec, ios::basefield);

    // Writing points
    fluentMeshFile
            << "(10 (3 1 ";

    fluentMeshFile.setf(ios::hex, ios::basefield);
    fluentMeshFile
        << nPoints() << " 1 3)"
        << std::endl << "(" << std::endl;

    fluentMeshFile.precision(10);
    fluentMeshFile.setf(ios::scientific);

    for (const auto& p : points())
    {
        fluentMeshFile
            << "    " << p.x() << " " << p.y() << " " << p.z() << '\n';
    }

    fluentMeshFile
        << "))" << std::endl << std::endl;

    const labelUList& own = owner();
    const labelUList& nei = neighbour();
    const auto& fcs = faces();

    // Writing (mixed) internal faces
    fluentMeshFile
        << "(13 (2 1 "
        << own.size() << " 2 0)" << std::endl << "(" << std::endl;

    forAll(own, facei)
    {
        const auto& l = fcs[facei];

        fluentMeshFile << "    ";
        fluentMeshFile << l.size() << " ";

        forAll(l, lI)
        {
            fluentMeshFile << l[lI] + 1 << " ";
        }

        fluentMeshFile << nei[facei] + 1 << " ";
        fluentMeshFile << own[facei] + 1 << std::endl;
    }

    fluentMeshFile << "))" << std::endl;

    label nWrittenFaces = own.size();

    // Writing boundary faces
    forAll(boundary(), patchi)
    {
        const faceUList& patchFaces = boundaryMesh()[patchi];

        const labelUList& patchFaceCells = boundaryMesh()[patchi].faceCells();

        // The face group will be offset by 10 from the patch label

        // Write header
        fluentMeshFile
            << "(13 (" << patchi + 10 << " " << nWrittenFaces + 1
            << " " << nWrittenFaces + patchFaces.size() << " ";

        nWrittenFaces += patchFaces.size();

        // Write patch type
        if (isA<wallFvPatch>(boundary()[patchi]))
        {
            fluentMeshFile << 3;
        }
        else if
        (
            isA<symmetryPlaneFvPatch>(boundary()[patchi])
         || isA<symmetryFvPatch>(boundary()[patchi])
        )
        {
            fluentMeshFile << 7;
        }
        else
        {
            fluentMeshFile << 4;
        }

        fluentMeshFile
            <<" 0)" << std::endl << "(" << std::endl;

        forAll(patchFaces, facei)
        {
            const auto& l = patchFaces[facei];

            fluentMeshFile << "    ";
            fluentMeshFile << l.size() << " ";

            // Note: In Fluent, all boundary faces point inwards, which is
            // opposite from the OpenFOAM convention.
            // Turn them around on printout
            forAllReverse(l, lI)
            {
                fluentMeshFile << l[lI] + 1 << " ";
            }

            fluentMeshFile << patchFaceCells[facei] + 1 << " 0" << std::endl;
        }

        fluentMeshFile << "))" << std::endl;
    }

    // Writing cells
    fluentMeshFile
        << "(12 (1 1 " << nCells() << " 1 0)" << nl
        << '(';

    const cellModel& hex = cellModel::ref(cellModel::HEX);
    const cellModel& prism = cellModel::ref(cellModel::PRISM);
    const cellModel& pyr = cellModel::ref(cellModel::PYR);
    const cellModel& tet = cellModel::ref(cellModel::TET);

    const cellShapeList& cells = cellShapes();

    label nHex = 0;
    label nPrism = 0;
    label nPyr = 0;
    label nTet = 0;
    label nPoly = 0;

    int nElemPerLine = 25;  // Start with linebreak and indent

    forAll(cells, celli)
    {
        if (nElemPerLine == 25)
        {
            // 25 elements per line with initial indent (readability)
            fluentMeshFile << "\n   ";
            nElemPerLine = 0;
        }
        else if (!(nElemPerLine % 5))
        {
            // Format in blocks of 5 (readability)
            fluentMeshFile << token::SPACE;
        }
        fluentMeshFile << token::SPACE;
        ++nElemPerLine;


        if (cells[celli].model() == tet)
        {
            fluentMeshFile << 2;
            ++nTet;
        }
        else if (cells[celli].model() == hex)
        {
            fluentMeshFile << 4;
            ++nHex;
        }
        else if (cells[celli].model() == pyr)
        {
            fluentMeshFile << 5;
            ++nPyr;
        }
        else if (cells[celli].model() == prism)
        {
            fluentMeshFile << 6;
            ++nPrism;
        }
        else
        {
            fluentMeshFile << 7;
            ++nPoly;
        }
    }

    fluentMeshFile
        << nl << "))" << nl;

    // Return to dec
    fluentMeshFile.setf(ios::dec, ios::basefield);

    // Writing patch types
    fluentMeshFile << "(39 (1 fluid fluid-1)())" << std::endl;
    fluentMeshFile << "(39 (2 interior interior-1)())" << std::endl;

    // Writing boundary patch types
    forAll(boundary(), patchi)
    {
        fluentMeshFile
            << "(39 (" << patchi + 10 << " ";

        // Write patch type
        if (isA<wallFvPatch>(boundary()[patchi]))
        {
            fluentMeshFile << "wall ";
        }
        else if
        (
            isA<symmetryPlaneFvPatch>(boundary()[patchi])
         || isA<symmetryFvPatch>(boundary()[patchi])
        )
        {
            fluentMeshFile << "symmetry ";
        }
        else
        {
            fluentMeshFile << "pressure-outlet ";
        }

        fluentMeshFile
            << boundary()[patchi].name() << ")())" << std::endl;
    }

    // Report some information.
    // NB: conversion is serial-only, so no need to reduce the values
    Info<< "Mesh had cells of these type:" << nl
        << "    hexahedra:  " << nHex << nl
        << "    prisms:     " << nPrism << nl
        << "    pyramids:   " << nPyr << nl
        << "    tetrahedra: " << nTet << nl
        << "    polyhedra:  " << nPoly << endl;
}


// ************************************************************************* //