Tutorial to set up a case for chtMultiRegionFoam in OpenFOAM 2.0.0

Tutorial to set up a case for
chtMultiRegionFoam in OpenFOAM
2.0.0
Arpit Singhal
University of Luxembourg
March 3, 2014
The OpenFOAM-solver chtMultiRegionFoam is meant to be used for heat-
transfer between a solid and a fluid originally. As it does work with different
regions of different properties, the setup is therefore different from the other
OpenFOAM cases.
This tutorial is written for setting up a basic case for chtMultiRegionFoam
(cMRF) in an Openfoam.
tutorial

Contents 1
Contents
1 Introduction 2
2 Basic Workﬂow 3
3 chtMRF Case Setup 4
3.1 Geometry and Mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4
3.2 Creating the Regions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5
3.2.1 Declaring the Regions . . . . . . . . . . . . . . . . . . . . . . . . 5
3.2.2 Deﬁning the Region by Zones . . . . . . . . . . . . . . . . . . . . 6
3.3 Splitting the Mesh . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7
3.4 Necessary Files and Folders . . . . . . . . . . . . . . . . . . . . . . . . . 8
3.4.1 Files setup by the user . . . . . . . . . . . . . . . . . . . . . . . . 9
3.4.2 Files setup by OpenFOAM utilities . . . . . . . . . . . . . . . . . 15
4 Running the case 18
5 Using scripting 18
6 Appendice 21
tutorial

1 Introduction 2
1 Introduction
What is meant by ”multiregion multi physics modeling”? It is inherently-coupled physics
on disparate continua (e.g. fluid, solid, different solids). In multiregion multi physics
separate governing equations for each continuum/region are solved, as shown in 1.1
seperate governing equations will be solved for Region 1 and Region 2 depending upon
their phase and Γ represents a region interface. A region can be defined as coherent
continum of the same phase.
Figure 1.1: Example
Generally two different approaches to solving such problems are distinguished:
• Monolithic: use same primitive variables, cast governing equations in terms of
these variables, solve a single coupled matrix equation system
• Partitioned: separate governing equations, solve separate matrix equation systems,
couple at the boundary interface, sub-iterate until coupled convergence is reached
Here, we focus on partitioned approaches using OpenFOAM’s multiregion function-
ality (conjugate heat/mass transfer). For a multiregion partitioned solver the working
steps are as follows:
1. Define multiple meshes, one for each ”region”
2. Create field variables on each mesh
3. Solve separate governing equations on each mesh
4. Multiregion coupling at the boundary interface between regions
5. Subiterate until fully-coupled solution is reached
tutorial

2 Basic Workflow 3
2 Basic Workflow
The basic work flow for a case setup is explained in fig. 2.1.
Create a Mesh of the full domain
Define regions inside the domain
by selecting cells (using cellSet)
Create cell zones from
the created cellSets
Split mesh into regions
according to defined zones
Basic work flow of a chtMultiRegion case
Run case
Prepare a general OpenFoam Case
Create patches and fields for all regions
changeDict
Define coupled patches
Define boundary conditions
Define region properties
Figure 2.1: The case visualization in 2D
tutorial

3 chtMRF Case Setup 4
3 chtMRF Case Setup
In this case we have four different regions (Air1, Air2, Solid1 and Solid2). The
case is a simple set up with warm solid parts (Solid1 and Solid2), which are subjected
to fluid parts (Air1 and Air2). In this case we are not taking into account any airflow
(i.e. there is no inlet or outlet airflow) but the buoyancy effects are considered, while
solving the case. There will be heat transfer taking place between the warm solid parts
and the fluid parts.
3.1 Geometry and Mesh
A graphical representation of the geometry can be seen in Fig. 3.1.
The geometry is defined and then meshed using the OpenFOAM blockMesh tool. After
Air2_to_Air1
Air1_to_Solid1
Air2_to_Solid2Solid1_to_Solid2
minX
maxY
maxX
minY
x
y
z
Air1_to_Solid2
Figure 3.1: The case visualization in 2D
running the blockMesh utility by typing
$ blockMesh
tutorial

3.2 Creating the Regions 5
the mesh is created as depicted in fig.3.2.
Figure 3.2: Mesh of the full domain
3.2 Creating the Regions
The regions are created in the domain depending upon their phases and they are created
on the basis of the zones defined.
3.2.1 Declaring the Regions
The regions and their property type are given in table 3.1.
Table 3.1: Table for region properties
Region Type
Air1 fluid
Solid1 solid
Air2 fluid
Solid2 solid
Every region has several patches for which boundary or coupling conditions have to
be specified. Thus, a patch can be of the following two types:
• boundary patch
tutorial

3.2 Creating the Regions 6
• coupling patch
A boundary patch is a regular type patch for which the user may define any possible
boundary condition available in OpenFOAM. Coupling patches are those patches where
the solutions of the different regions are coupled. A coupling patch belongs to a so-
called coupled patch pair. Such a pair consists of coinciding patches, one associated with
each region. Table 3.2 lists all patches, the region they belong to and their type for the
presented case.
Table 3.2: Table of patches
Patch Regions Type
minX Air1, Solid1 boundary patch
maxX Air2, Solid2 boundary patch
minY Solid1, Solid2 boundary patch
maxY Air1, Air2 boundary patch
minZ Air1, Air2, Solid1, Solid2 boundary patch
maxZ Air1, Air2, Solid1, Solid2 boundary patch
Solid1 to Solid2 Solid1, Solid2 coupling patch
Air1 to Solid1 Solid1, Air1 coupling patch
Air1 to Solid2 Air1, Solid2 coupling patch
Air1 to Air2 Air1, Air2 coupling patch
Air2 to Solid2 Air2, Solid2 coupling patch
3.2.2 Defining the Region by Zones
In the presented case the following regions must be created: Air1, Air2, Solid1 and
Solid2. In order to create these regions the domain is divided into zones. To do so a
subset of cells within the domain is selected to form a so-called cellSet. A cellSet is a
random selection of cells from the domain, whereas a zone is a coherent subset of cells
which finally can be used to define a region. According to the cellSets four zones are
defined which mark the different regions.
In order to define cellSets and cellZones a OpenFOAM commandline utility called setSet
(topoSet in newer versions of OpenFOAM) is used. This tool requires a dictionary-file as
input. Thus, within the case folder a file ending with .setSet must exist, which contains
the settings used to define the different cellSets/cellZones/regions in the domain. The
following command starts the utility with the dictionary file that contains the commands
to be executed.
tutorial

3.3 Splitting the Mesh 7
$ setSet −batch makeCellSets . setSet
An example of the dictionary file of the presented case is attached for simplicity (Listing
1).
Listing 1: Extract from makeCellSets.setSet
1 c e l l S e t Solid1 new boxToCell (0 0 0 )(10 0.3 1)
cellZoneSet Solid1 new setToCellZone Solid1
c e l l S e t Solid2 new boxToCell (10 0 0 )(20 0.5 1)
5 cellZoneSet Solid2 new setToCellZone Solid2
c e l l S e t Air1 new boxToCell (0 0.3 0 )(10 1 1)
cellZoneSet Air1 new setToCellZone Air1
10 c e l l S e t Air2 new boxToCell (10 0.5 0 )(20 1 1)
cellZoneSet Air2 new setToCellZone Air2
The first two lines used in the .setSet file are briefly explained as:
c e l l S e t Solid1 new boxToCell (0 0 0) (10 0.3 1)
This creates a new cellSet from a selection of cells. The new action shows it will
be a new set. The name of the cellSet is Solid1 and the source for the cellSet-function
is the boxToCell function. The numbers in brackets are parameters to the boxToCell-
function: All cells contained within the rectangular box spanning between the points
with coordinates (0 0 0) and (10 0.3 1) are selected for the cellSet Solid1. The line
cellZoneSet Solid1 new setToCellZone Solid1
builds a cellZoneSet from an existing cellSet (here using Solid1). Thus, within the
original domain a new zone has been created as depicted in fig.3.3.
This can be repeated in order to define the desired zones representing regions within
the domain.
3.3 Splitting the Mesh
After the user has defined all necessary regions by creating zones for them as described in
the previous section the mesh of the domain has to be split into several disjoint meshes.
Note that the originally created mesh of the full domain will be used within the regions.
tutorial

3.4 Necessary Files and Folders 8
Figure 3.3: Zone created by cellZone from the entire domain
Thus, proper grid resolution for the regional meshes must already be accounted for when
creating the mesh of the full domain.
$ splitMeshRegions −cellZones −overwrite
The splitted mesh can be checked/visualized in paraview using the command as shown
in the listing3.3 for Air1
$ paraFoam −touch −region Air1
Then in paraview, *.OpenFoam file should be loaded and can be visualized. The splitted
mesh is shown in fig. 3.4.
3.4 Necessary Files and Folders
A typical OpenFOAM case directory consists of the following three folders:
• 0
• constant
• system
This general case structure is also kept for multiregion cases. The final correct setup of
a multiregion case is shown in fig.3.5. Note that for each region a subdirectory containing
tutorial

Figure 3.4: Splitted mesh
the information for the particular region exists. Some of the files are manually created
by the user while others are created by the OpenFOAM utilities. It is explained in the
further sections in detail.
In the following sections details about the individual directories will be given.
3.4.1 Files setup by the user
When starting a new multiregion case the directories and their content highlighted in
fig. 3.6 must be created manually by the user according to the problem definition.
0 directory: First, manually bring in the necessary field files as usual. For a chtMulti-
RegionFoam case it is necessary to have files for:epsilon, k, p, p rgh, T, U, Ychar and Ypmma.
These files are identical to what one would find in any other chtMultiRegionFoam case
/0-directory.
For the solid regions:T, Ychar and Ypmma are necessary, whereas for the fluid regions:epsilon, g, k,
are the required files.
constant directory: As is any standard OpenFOAM case, the constant folder must
contain a standard polymesh directory, including a standard blockMeshDict-file, which
tutorial

Figure 3.5: Final case structure of a multiregion case before running the solver
tutorial

Files for all desired fields
have to be created inside
0 directory by the user.
Folders for each region must
be created by the user. They
should contain default files for
any fluid and solid.
Defines the geometry and
mesh the full domain.
Defines desired regions
and their property.
Folders for each region must
be created by the user. They
should contain default files
for any fluid and solid. The
user must add and edit the
changeDictionaryDict
Figure 3.6: Case structure as prepared by the user before running scripts
tutorial

created by splitMesh:
For each region a folder
is created inside the
0 folder and all originally
field files from the 0
folder are copied into the
region folders
created by splitMesh:
The mesh is splitted into
the different regions and
for every region a
separate mesh is defined.
created by changeDict:
This file defines all the
patches of a particular
region.
modified by changeDict:
boundary, initial and
coupling conditions for all
fields are modified according
to the changeDictionaryDict
file of the region
Figure 3.7: Files and directories created by OpenFOAM utilities
tutorial

defines the full domain and its mesh.
In contrast to a standard case, the files defining the other properties have to go into the
different regional folders, i.e. transportProperties and thermophysicalProperties
within the folders for fluid regions and solidThermophysicalProperties within the
folders for the solid regions as shown in listing3 and listing4 .
Within the constant-folder it is necessary to produce all the region folders. Addition-
ally within the constant folder it also is necessary to build (or copy from elsewhere) a
file called regionProperties. This file assigns the physical phase to each region: Either
fluid or solid. An example for this file can be seen in the listing 2.
Listing 2: Extract from regionProperties
// ∗ ∗ ∗ ∗ ∗ ∗ ∗ ∗ ∗ ∗ ∗ ∗ ∗ ∗ ∗ ∗ ∗ ∗ //
fluidRegionNames ( air1 air2 ) ;
solidRegionNames ( s o l i d 1 s o l i d 2 ) ;
// ∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗∗ //
Inside the solver fluidRegions and solidRegions are treated differently by solving
different governing equations for each phase.
For the fluid regions the default constant files should be included from any chtMulti-
RegionFoam case/constant file. For the fluid regions, the fluid region should contain a
thermophysicalProperties file containing the properties of the fluid in the fluid region.
Like the Air1 thermophysicalProperties file contains:
Listing 3: Extract from Air1 thermophysicalProperties file
mixture
{
specie
{
nMoles 1;
molWeight 2 8 . 9 ;
}
thermodynamics
{
tutorial

Cp 1000;
Hf 0;
}
transport
{
mu 1.8 e −05;
Pr 0 . 7 ;
}
}
Similarly for solid regions a solidThermophysicalProperties must exist with the
folder of the region, an example of such a solidThermophysicalProperties is given
for Solid1:
Listing 4: Extract from Solid1 solidThermophysicalProperties ﬁle
constSolidThermoCoeffs
{
//− thermo properties
rho rho [1 −3 0 0 0 0 0] 8000;
Cp Cp [0 2 −2 −1 0 0 0] 450;
K K [1 1 −3 −1 0 0 0] 80;
//− radiation properties
kappa kappa [0 −1 0 0 0 0 0] 0;
sigmaS sigmaS [0 −1 0 0 0 0 0] 0;
emissivity emissivity [0 0 0 0 0 0 0] 0;
//− chemical properties
Hf Hf [0 2 −2 0 0 0 0] 0;
}
.
.
.
. . . . . .
. .
}
tutorial

system directory: In the system directory, once again set up the folders for the regions.
In each region folder there should be a changeDictionaryDict file, which contains
details about the necessary fields in the region like T, U, etc.
Get a working controlDict file, for example from any tutorial into this folder. Af-
terwards get a dummy fvSchemes file. This one is the same as any other fvSchemes,
except for the different functions containing no values between the curly brackets. Fur-
theron one has to get a fvSolution which only defines the outer correctors into this
folder. It is optional to get a decomposeParDict file in case one opts for running parallel
computations. For all of the different regional folders: Get a decomposeParDict file
and get full fvSchemes and fvSolution files into the folders. For the latter ones, keep
in mind that they will be different for the fluids and for the solids.
3.4.2 Files setup by OpenFOAM utilities
Most of the necessary case files and folder (This is highlighted in 3.7 for the different
regions are created by automated generation using scripts and OpenFOAM utilities.
The most important OpenFOAM utilities for a multiregion case are:
splitMesh creates the polyMesh directories and their content within the constant/regionXYZ/
folders;
additionally it creates 0/regionXYZ/ directories for all regions and copies all the
field files existing in the 0 directory into the 0/regionXYZ/ directories
changeDictionary uses changeDictionaryDict files located in system/regionXYZ/ fold-
ers to create initial, boundary and coupling conditions for all fields existing in
0/regionXYZ/ directory for all regions
0 directory: During execution of splitMesh the user created field files are copied to
the region subdirectories. As a next step unnecessary fields are removed for some regions
(see extract given in Listing 5) and only those being part of the governing equations are
kept (for example solids are assumed to be stationary, thus no velocity field is required).
Listing 5: Extract from Allrun script
# remove f l u i d f i e l d s from s o l i d regions
for i in s o l i d 1 s o l i d 2
do
rm −f 0∗/ $i /{mut , alphat , epsilon , k , p ,U, p rgh}
tutorial

done
# remove s o l i d f i e l d s from f l u i d regions
for i in air1 air2
do
rm −f 0∗/ $i /{Ychar ,Ypmma}
done
Now the initial, boundary and coupling conditions for all fields in every region have to
be specified appropriately. In order to do so the commandline utility changeDictionary
is used. For example for the region Air1 the following line must be executed:
$ changeDictionary −region Air1 > log . changeDictionary . Air1 2>&1
The utility expects a file called changeDictionaryDict to exist within the folder system/Air/.
Initial and coupling condition of the regions are defined with in changeDictionaryDict.
Boundary conditions for the boundaries on the outside of the complete simulation do-
main and boundary conditions or so-called coupling conditions for any of the coupling
patches between the regions are built using the following scheme: For example for region
Air1 in the changeDictionaryDict file contains the following code for the T field:
T
{
i n t e r n a l F i e l d uniform 300;
boundaryField
{
”.∗”
{
type zeroGradient ;
}
” a i r 1 t o .∗”
{
type compressible : : turbulentTemperatureCoupledBaffleMixed ;
neighbourFieldName T;
. . .
}
tutorial

}
}
In this example the boundary patches are all treated the same (using a wildcard ".*")
and are given the boundary conditions of type zeroGradient. For the coupling patch
there is special kind of boundary condition required (here
compressible::turbulentTemperatureCoupledBaffleMixed).
The keyword neighbourFieldName indicates that the T field of air1 is coupled to the
T field of the other regions.
Similarly for all other regions, the initial, boundary and coupling conditions must be
taken care of.
In each of the region folders a file called cellToRegion is created during execution of
the changeDictionaryDict command. The content of these files are like any other
field file but not associated to a specific field. The BC type is either zeroGradient or
calculated. Possibly other parameters would work as well, but only these have been
tested. In any case every coupling patches to other regions have to be defined of type
calculated whereas boundary patches (to outside of domain) are of type zeroGradient.
for Air1 the entry used is shown by listing 6
Listing 6: Extract from cellToRegion
boundaryField
{
maxY
{
type zeroGradient ;
}
minX
{
type zeroGradient ;
}
minZ
{
type zeroGradient ;
}
maxZ
tutorial

4 Running the case 18
{
type zeroGradient ;
}
a i r 1 t o a i r 2
{
type calculated ;
value uniform 0;
}
a i r 1 t o s o l i d 2
{
type calculated ;
value uniform 0;
}
a i r 1 t o s o l i d 1
{
type calculated ;
value uniform 0;
}
}
constant directory: In the constant folder, the splitMesh utility creates a seperate
mesh for each region. This can be seen in the fig. 3.7
4 Running the case
After following each step as defined in the above tutorial. The case can be executed by
using the command in the terminal as depicted in the listing. 4
$ chtMultiRegionFoam
5 Using scripting
An Allrun can be explained as a script file which contains all the commands used to
execute the case, for example in this case the Allrun used can be seen as in Listing
tutorial

shown in 5.1. So just executing the Allrun will now run the case, instead of typing each
command seperately in the terminal.
tutorial

Figure 5.1: Allrun script
tutorial

6 Appendice 21
6 Appendice
Listing 7: Extract from Allrun
#!/bin/sh
cd ${0%/∗} | | exit 1 # run from t h i s directory
RUNPAR=”YES” ;
# Source t u t o r i a l run functions
. $WM PROJECT DIR/bin/ t o o l s /RunFunctions
# −−− (A) −− Defining geometry and mesh of f u l l domain
runApplication blockMesh
# −−− (B) −− Creating the regions in two steps :
# 1) defining c e l l S e t s
# 2) creating cellZones which define the regions
runApplication setSet −batch makeCellSets . setSet
# −−− (C) −− S p l i t t i n g the mesh according to the defined regions
runApplication splitMeshRegions −cellZones −overwrite
exit
# −−− (D) −− Remove unnecessary f i e l d f i l e s from regions
#
# −−−− (D. 1 ) − Remove f l u i d f i e l d s from s o l i d regions
for i in s o l i d 1 s o l i d 2
do
rm −f 0∗/ $i /{mut , alphat , epsilon , k , p ,U, p rgh}
done
tutorial

6 Appendice 22
# −−−− (D. 2 ) − Remove s o l i d f i e l d s from f l u i d regions
for i in air1 air2
do
rm −f 0∗/ $i /{Ychar ,Ypmma}
done
# −−− (E) −− Define i n i t i a l , boundary and coupling conditions
# for a l l f i e l d s
# of a l l regions
#
# loop over regions
for i in air1 air2 s o l i d 1 s o l i d 2
do
changeDictionary −region $i > log . changeDictionary . $i 2>&1
done
# −−− (F) −− RUN case
# choose between PARALLEL or SEQUENTIAL RUN
i f [ ”$RUNPAR” = ”YES” ] ;
then
echo ’ −−− Running in p a r a l l e l mode ’ ;
# Decompose
do
decomposePar −region $i > log . decomposePar . $i 2>&1
done
# Run
mpirun . openmpi −np 4 chtMultiRegionFoam −p a r a l l e l > log
# Reconstruct
tutorial

6 Appendice 23
do
reconstructPar −region $i > log . reconstructPar . $i2 >&1
done
e l s e
echo ’ −−− Running in sequential mode ’ ;
#−− Run on s i n g l e processor
chtMultiRegionFoam > log
f i
echo
echo ” creating f i l e s for paraview post−processing ”
echo
for i in s o l i d 1 s o l i d 2 air1 air2
do
paraFoam −touch −region $i
done
# −−−−−−−−−−−−−−−−−− end−of−f i l e
tutorial

Tutorial to set up a case for chtMultiRegionFoam in OpenFOAM 2.0.0

More Related Content

What's hot (20)

Viewers also liked (17)

Similar to Tutorial to set up a case for chtMultiRegionFoam in OpenFOAM 2.0.0 (6)

Recently uploaded (20)

Tutorial to set up a case for chtMultiRegionFoam in OpenFOAM 2.0.0