The user can generate meshes using other packages and convert them into the
format that OpenFOAM uses. The mesh conversion codes have the naming
convention available mesh converters are:
fluentMeshToFoam
reads a Fluent.msh mesh file, working for both 2-D and
3-D cases;
Fluent writes mesh data to a single file with a .msh extension. The
file must be written in ASCII format, which is not the default option in
Fluent. It is possible to convert single-stream Fluent meshes, including the 2
dimensional geometries. In OpenFOAM, 2 dimensional geometries are
currently treated by defining a mesh in 3 dimensions, where the front
and back plane are defined as the empty boundary patch type. When
reading a 2 dimensional Fluent mesh, the converter automatically extrudes
the mesh in the third direction and adds the empty patch, naming it
frontAndBackPlanes.
The following features should also be observed.
The OpenFOAM converter will attempt to capture the Fluent boundary
condition definition as much as possible; however, since there is no clear,
direct correspondence between the OpenFOAM and Fluent boundary
conditions, the user should check the boundary conditions before
running a case.
Creation of axi-symmetric meshes from a 2 dimensional mesh is
currently not supported but can be implemented on request.
Multiple material meshes are not permitted. If multiple fluid materials
exist, they will be converted into a single OpenFOAM mesh; if a solid
region is detected, the converter will attempt to filter it out.
Fluent allows the user to define a patch which is internal to the mesh,
i.e. consists of the faces with cells on both sides. Such patches are not
allowed in OpenFOAM and the converter will attempt to filter them
out.
There is currently no support for embedded interfaces and refinement
trees.
The procedure of converting a Fluent.msh file is first to create a new
OpenFOAM case by creating the necessary directories/files: the case directory
containing a controlDict file in a system subdirectory. Then at a command prompt
the user should execute:
fluentMeshToFoam<meshFile>
where <meshFile> is the name of the .msh file, including the full or relative
path.
This section describes how to convert a mesh generated on the STAR-CD code
into a form that can be read by OpenFOAM mesh classes. The mesh can be
generated by any of the packages supplied with STAR-CD, i.e.PROSTAR, SAMM,
ProAM and their derivatives. The converter accepts any single-stream mesh
including integral and arbitrary couple matching and all cell types are supported.
The features that the converter does not support are:
multi-stream mesh specification;
baffles, i.e. zero-thickness walls inserted into the domain;
partial boundaries, where an uncovered part of a couple match is
considered to be a boundary face;
sliding interfaces.
For multi-stream meshes, mesh conversion can be achieved by writing each individual
stream as a separate mesh and reassemble them in OpenFOAM.
OpenFOAM adopts a policy of only accepting input meshes that conform to
the fairly stringent validity criteria specified in 5.1. It will simply not run using
invalid meshes and cannot convert a mesh that is itself invalid. The following
sections describe steps that must be taken when generating a mesh using a mesh
generating package supplied with STAR-CD to ensure that it can be converted to
OpenFOAM format. To avoid repetition in the remainder of the section, the mesh
generation tools supplied with STAR-CD will be referred to by the collective name
STAR-CD.
We strongly recommend that the user run the STAR-CD mesh checking tools
before attempting a starToFoam conversion and, after conversion, the checkMesh
utility should be run on the newly converted mesh. Alternatively, starToFoam may
itself issue warnings containing PROSTAR commands that will enable the
user to take a closer look at cells with problems. Problematic cells and
matches should be checked and fixed before attempting to use the mesh with
OpenFOAM. Remember that an invalid mesh will not run with OpenFOAM, but
it may run in another environment that does not impose the validity
criteria.
Some problems of tolerance matching can be overcome by the use of a
matching tolerance in the converter. However, there is a limit to its effectiveness
and an apparent need to increase the matching tolerance from its default level
indicates that the original mesh suffers from inaccuracies.
When mesh generation in is completed, remove any extraneous vertices and
compress the cells boundary and vertex numbering, assuming that fluid cells have
been created and all other cells are discarded. This is done with the following
PROSTAR commands:
CSET NEWS FLUID CSET INVE
The CSET should be empty. If this is not the case, examine the cells in CSET and
adjust the model. If the cells are genuinely not desired, they can be removed using
the PROSTAR command:
CDEL CSET
Similarly, vertices will need to be discarded as well:
CSET NEWS FLUID VSET NEWS CSET VSET INVE
Before discarding these unwanted vertices, the unwanted boundary faces have to
be collected before purging:
If the BSET is not empty, the unwanted boundary faces can be deleted using:
BDEL BSET
At this time, the model should contain only the fluid cells and the supporting
vertices, as well as the defined boundary faces. All boundary faces should be fully
supported by the vertices of the cells, if this is not the case, carry on cleaning the
geometry until everything is clean.
By default, STAR-CD assigns wall boundaries to any boundary faces not
explicitly associated with a boundary region. The remaining boundary faces are
collected into a default boundary region, with the assigned boundary type 0.
OpenFOAM deliberately does not have a concept of a default boundary
condition for undefined boundary faces since it invites human error, e.g. there is
no means of checking that we meant to give all the unassociated faces the default
condition.
Therefore all boundaries for each OpenFOAM mesh must be specified for a
mesh to be successfully converted. The default boundary needs to be
transformed into a real one using the procedure described below:
Plot the geometry with Wire Surface option.
Define an extra boundary region with the same parameters as the default
region 0 and add all visible faces into the new region, say 10, by selecting a
zone option in the boundary tool and drawing a polygon around the entire
screen draw of the model. This can be done by issuing the following
commands in PROSTAR:
RDEF 10 WALL BZON 10 ALL
We shall remove all previously defined boundary types from the set. Go
through the boundary regions:
BSET NEWS REGI 1 BSET NEWS REGI 2 ... 3, 4, ...
Collect the vertices associated with the boundary set and then the boundary
faces associated with the vertices (there will be twice as many of them as in
the original set).
BSET NEWS REGI 1 VSET NEWS BSET BSET NEWS VSET ALL BSET DELE REGI 1 REPL
This should give the faces of boundary Region 10 which have been defined
on top of boundary Region 1. Delete them with BDEL BSET. Repeat these for
all regions.
BSET NEWS VSET ALL BSET INVE (Should be empty also!) BSET INVE BCOM BSET
CHECK ALL GEOM
Internal PROSTAR checking is performed by the last two commands,
which may reveal some other unforeseeable error(s). Also, take note of the
scaling factor because PROSTAR only applies the factor for STAR-CD
and not the geometry. If the factor is not 1, use the scalePoints utility in
OpenFOAM.
Once the mesh is completed, place all the integral matches of the model into
the couple type 1. All other types will be used to indicate arbitrary matches.
CPSET NEWS TYPE INTEGRAL CPMOD CPSET 1
The components of the computational grid must then be written to their own
files. This is done using PROSTAR for boundaries by issuing the command
BWRITE
by default, this writes to a .23 file (versions prior to 3.0) or a .bnd file (versions 3.0
and higher). For cells, the command
CWRITE
outputs the cells to a .14 or .cel file and for vertices, the command
VWRITE
outputs to file a .15 or .vrt file. The current default setting writes the files in
ASCII format. If couples are present, an additional couple file with the extension
.cpl needs to be written out by typing:
CPWRITE
After outputting to the three files, exit PROSTAR or close the files. Look
through the panels and take note of all STAR-CD sub-models, material and
fluid properties used - the material properties and mathematical model
will need to be set up by creating and editing OpenFOAM dictionary
files.
The procedure of converting the PROSTAR files is first to create a new
OpenFOAM case by creating the necessary directories. The PROSTAR files
must be stored within the same directory and the user must change the
file extensions: from .23, .14 and .15 (below STAR-CD version 3.0), or
.pcs, .cls and .vtx (STAR-CD version 3.0 and above); to .bnd, .cel and .vrt
respectively.
The .vrt file is written in columns of data of specified width, rather than free
format. A typical line of data might be as follows, giving a vertex number followed
by the coordinates:
The starToFoam converter reads the data using spaces to delimit the ordinate
values and will therefore object when reading the previous example. Therefore,
OpenFOAM includes a simple script, foamCorrectVrt to insert a space between
values where necessary, i.e. it would convert the previous example to:
The translator utility starToFoam can now be run to create the boundaries,
cells and points files necessary for a OpenFOAM run:
starToFoam<meshFilePrefix>
where <meshFilePrefix> is the name of the the prefix of the mesh files,
including the full or relative path. After the utility has finished running,
OpenFOAM boundary types should be specified by editing the boundary file by
hand.
GAMBIT writes mesh data to a single file with a .neu extension. The procedure
of converting a GAMBIT.neu file is first to create a new OpenFOAM case, then at
a command prompt, the user should execute:
gambitToFoam<meshFile>
where <meshFile> is the name of the .neu file, including the full or relative
path.
The GAMBIT file format does not provide information about type of the
boundary patch, e.g. wall, symmetry plane, cyclic. Therefore all the patches
have been created as type patch. Please reset after mesh conversion as
necessary.
OpenFOAM can convert a mesh generated by I-DEAS but written out in
ANSYS format as a .ans file. The procedure of converting the .ans file is first to
create a new OpenFOAM case, then at a command prompt, the user should
execute:
ideasToFoam<meshFile>
where <meshFile> is the name of the .ans file, including the full or relative
path.
CFX writes mesh data to a single file with a .geo extension. The mesh format
in CFX is block-structured, i.e. the mesh is specified as a set of blocks with
glueing information and the vertex locations. OpenFOAM will convert the mesh
and capture the CFX boundary condition as best as possible. The 3 dimensional
‘patch’ definition in CFX, containing information about the porous, solid regions
etc. is ignored with all regions being converted into a single OpenFOAM mesh.
CFX supports the concept of a ‘default’ patch, where each external face without a
defined boundary condition is treated as a wall. These faces are collected by the
converter and put into a defaultFaces patch in the OpenFOAM mesh
and given the type wall; of course, the patch type can be subsequently
changed.
Like, OpenFOAM 2 dimensional geometries in CFX are created as 3
dimensional meshes of 1 cell thickness [**]. If a user wishes to run a 2 dimensional
case on a mesh created by CFX, the boundary condition on the front and back
planes should be set to empty; the user should ensure that the boundary
conditions on all other faces in the plane of the calculation are set correctly.
Currently there is no facility for creating an axi-symmetric geometry from a 2
dimensional CFX mesh.
The procedure of converting a CFX.geo file is first to create a new
OpenFOAM case, then at a command prompt, the user should execute:
cfxToFoam<meshFile>
where <meshFile> is the name of the .geo file, including the full or relative
path.
