OpenFOAM-6/etc/templates/singleFluidCHT

Overview
========
+ This is a template case for conjugate heat transfer (CHT)
+ It is designed to work specifically with the foamSetupCHT utility
+ The template works simply for cases with a single fluid region and multiple
  solid regions; it can be adapted for cases with multiple fluid regions
+ It is setup to run the chtMultiRegionFoam solver
+ The Allmesh and Allrun scripts demonstrate the commands to be run

Meshing Strategy
================
+ A single mesh is first created for the entire fluid/solid domain, including
  relevant boundary patches, with cellZones to describe the solid regions.
+ The single mesh is then split into separate meshes for each region using
  splitMeshRegions.
+ The case is designed to be meshed with snappyHexMesh
+ The overall (comined fluid/solid) domain is described by a single a surface
  geometry file named (default name "CAD.obj"), that includes separate surface
  regions to describe boundary patches
+ A surface geometry file is provided for each solid; the template includes
  example entries for a single solid with geometry file "solid.obj".

Surface Geometry
================
+ Copy the overall domain geometry file ("CAD.obj") and solid geometry files
  (e.g. "solid.obj") to the constant/triSurface
+ The CAD.obj should contain an inlet and outlet region to create the relevant
  patches in the mesh

Background Mesh
===============
+ The user should establish the bounds of their "CAD.obj" file
+ The blockMeshDict file contains a backgroundMesh subditionary
+ For internal flows, where "CAD.obj" describes the external boundary, set xMin,
  xMax, etc to be beyond the "CAD.obj" bounds
+ For external flows, the background mesh can define the external boundary by
  uncommenting entries, e.g. left, in the boundary section of blockMeshDict
+ Set background mesh density with xCells, yCells, zCells
+ Run blockMesh

Features
========
+ Edit the surfaceFeatures file to include all the surface geometry files
+ Run surfaceFeatures to extract features for explicit feature capturing

Castellated Mesh
================
+ In the snappyHexMeshDict file, configure the "geometry" subdictionary to
  include an entry for each surface geometry file, e.g. "CAD.obj", "solid.obj"
+ Replace <inletPatch> with the name of the inlet region in the "CAD.obj" file
+ Replace <outletPatch> with the name of the outlet region
+ In refinementSurfaces, include an entry to create a cellZone for each solid
+ run snappyHexMesh to obtain a castellatedMesh
+ Review the mesh; modify refinement levels and regenerate the mesh as required
  (levels are set in refinementSurfaces and refinementRegions)

Snapped Mesh
============
+ In snappyHexMeshDict, set castellatedMesh off; snap on;
+ Run the snapping phase of snappyHexMesh
+ Review the mesh

Layers
======
+ To add layers to the mesh along wall boundary patches...
+ Switch on addLayers; switch snap off;
+ Run snappyHexMesh
+ The number of layers can be changed by modifying nSurfaceLayers

Creating the CHT Mesh
=====================
Run splitMeshRegions with "-cellZones" to split the solid cellZones into
separate mesh regions; the remaining fluid region can be named with the
"-defaultRegionName" option.  For example, to name the default region "fluid":

  splitMeshRegions -cellZones -defaultRegionName fluid -overwrite

Initialisation
==============
+ The case initialisation is performed largely by the foamSetupCHT utility
+ foamSetupCHT requires the user to configure a materialProperties file
  that includes entries for each region with
  + type : fluid or solid
  + material : e.g. air, aluminium, selected from configured materials in
    templates/materials directory
+ The user then runs foamSetupCHT which generates the region directories
  in 0, system and constant, containing the respective field, configuration and
  properties files
+ The user should edit these files accordingly.  The default models and
  configuration (e.g. fvSchemes) for each region are generally reliable, but
  the user must pay attention to field files (U, T, k, omega, etc), in
  particular the boundary conditions and initial conditions.
+ Region boundaries, e.g. solid-fluid and solid-solid, use the "wall" group
  boundary conditions by default.  External wall boundaries are part of the
  "externalWall" group, which has its own boundary condition settings
+ For convenience, some field data common to multiple regions, e.g. initial
  temperature, are provided through an "initialConditions" file

Source Terms
============
+ An fvOptions file is included in system for the solid regions
+ It contains examples of fixed temperature and heat flux sources which can
  be switched on accordingly

Running the Solver
==================
+ The case uses chtMultiRegionFoam which can run either as a steady-state
  solver, or as a transient solver.
+ The default setup is to run steady-state
+ To run transient, the user needs to modify the controlDict file, and fluid
  and solid fvSchemes and fvSolutions files.  The latter files are annotated
  with some information to remind users of the changes required.

Post-Processing
===============
+ In order to post-process with ParaView, run "paraFoam -touchAll", then open
  paraview and open the individual ".OpenFOAM" dummy files for individual mesh
  regions.