mirror of
https://github.com/OpenFOAM/OpenFOAM-6.git
synced 2025-12-08 06:57:46 +00:00
a863335743
The template is designed to work with the new foamSetupCHT utility. It works simply for cases with a single fluid region (and multiple solid regions); it can also be adapted for cases with multiple fluid regions. For more information see the included README file.
119 lines
5.2 KiB
Plaintext
119 lines
5.2 KiB
Plaintext
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.
|