CFD-Post has limited support for reading Common Fluids Format (CFF) files, which are written by some Ansys solvers, for example those of Ansys Fluent and Ansys CFX.
CFF data is supplied within a number of files that include:
At least one case file (extension ".cas.XXX", where "XXX" is solver-specific).
A case file includes the mesh and physics settings such as the definitions of domains and boundary conditions. It may also contain additional data depending on the solver that wrote the file.
A case file contains no reference to the associated results data file(s). However, if there is exactly one results data file in the same directory as a case file, and if it has the same file name (excluding the extension), CFD-Post will assume that the results file is associated with the case file.
At least one results data file (extension ".dat.XXX", where "XXX" is solver-specific).
A results data file contains the solution data and other output data. It also contains a reference to its associated case file.
(Typically) a fluids project file (extension .flprj).
The project file contains information that is used for transient postprocessing and file associations when sequences of files are supplied. Note that some solvers provide the files referenced by the .flprj file in a subdirectory named the same as the .flprj file without the file type extension.
The solver-specific part of the file extension is generally ".h5" for Fluent and ".cff" for CFX.
The recommended way to load CFF files into CFD-Post is to load the fluids project file. This is especially important for solutions that involve multiple case and data files, which must be loaded in the correct sequence. If you do not have the fluids project file, then you can load either the results data file or the case file:
If you load a results data file, the corresponding case file will also be loaded. This is especially useful when there is more than one results data file for a given case file.
If you load a case file, then CFD-Post will check to see if there is exactly one corresponding results data file; if there is, it will also be loaded.
The following topics are discussed:
The following topics are discussed:
- 8.15.6.1.1. Physical Objects (Domains, Boundary Conditions and Subdomains)
- 8.15.6.1.2. Topological Regions
- 8.15.6.1.3. Meshes
- 8.15.6.1.4. Mesh Zones
- 8.15.6.1.5. Steady State and Transient simulations
- 8.15.6.1.6. Multi-configuration (Modified Mesh/Modified Physics)
- 8.15.6.1.7. Single-phase and Multi-phase Solutions
- 8.15.6.1.8. Naming of Variables
When supplied, physical objects, such as those listed above, are shown in the CFD-Post tree as objects and their geometries are shown in the CFD-Post viewer. Normal operations can be carried out on these objects.
Physical objects are user-defined.
Physical objects are defined in terms of Topological Regions that are, in turn, defined in terms of the mesh (see Meshes).
Names of physical objects are preserved as supplied except when they don't conform with naming requirements, in which case they are automatically translated to conform (see Name Limitations in CFD-Post).
Topological regions are groups of one or more Mesh Zones (see below), normally of the same dimensionality
Topological regions are read from the file but are normally not displayed because physical objects are preferred. However, if physical objects such as domains and boundary conditions are not supplied, the topological regions are displayed.
In the case where neither physical objects nor topological regions are supplied by the file, the underlying mesh zones are displayed (see Mesh Zones).
Meshes can be defined in 2D (Axisymmetric and Planar) and 3D. Both can be read by CFD-Post.
Meshes might be defined in two forms: one that explicitly defines the cells and faces in terms of vertices; one where only the faces are defined in terms of vertices and the cell definition must be derived from the faces.
In CFD-Post, 2D meshes are extruded to 3D meshes. The extruded distance might not be identical to that seen when previous file formats are read.
Meshes are defined in terms of collections of cells, faces and nodes known as zones. Note: These are not be confused with solver zones.
Unless neither physical objects nor topological regions are supplied, mesh zones will not be presented in the user interface because it is unlikely that they have any physical significance.
Both steady state and transient simulations can be read by CFD-Post.
In the case of transient simulations, CFD-Post can only read simulations using a fluids project file that defines the order of the time steps.
Solver Timestep, Time, Crank Angle and other information might be read from the fluids project file depending on what is supplied by the solver.
Note: Timesteps are not displayed if they cannot be successfully loaded and validated.
Limited support is available for multi-configuration runs obtained from CFX-Solver cases.
Multi-configuration runs from Fluent are supported.
Note: Some transient cases loaded from Fluent or CFX may be discovered to be multi-configuration on read when they are not truly multi-configuration. This does not have a major impact on postprocessing.
Supported by CFD-Post
Where possible, CFD-Post uses the phase name supplied by the solver (see Name Limitations in CFD-Post).
Most solvers supply results variables using their native naming convention. Some of these variables have been translated to follow CFD-Post naming conventions for backwards compatibility.
It is possible to alter the naming convention used by CFD-Post by using the option in Edit > Options > CFD-Post > Files > Variables > Common File Format. By default, the convention is that of CFD-Post.
When the Native naming convention is used, CFD-Post uses the variable name supplied by the solver.
Species names are preserved where possible (see Name Limitations in CFD-Post). This may mean that the names differ from those seen in previous file formats.
Note that not all of the data available in other file formats is necessarily available in CFF files. The documentation of a solver that writes CFF files might mention limitations on which data it writes to CFF files.
Note: The HDF5 version used in 2024 R2 will result in failure when the
underlying file system does not support file locking, or where locks have been disabled.
To disable all file locking operations, create an environment variable named
HDF5_USE_FILE_LOCKING and set the value to the five-character string
FALSE.
CFD-Post has limitations for reading and using the data contained in CFF files:
CFD-Post does not support reading CFF files that were written by Ansys solvers older than Release 2020 R2.
CFD-Post does not support reading CFF files that were written by Ansys solvers other than CFX-Solver or Fluent.
CFD-Post offers limited or no functionality in these general areas:
Derived variables (limited support)
Results loaded into CFD-Post can show differences in variable values at specific locations depending on the data source. For example, there can be differences in derived variable values between CFF files and legacy files.
Axis of rotation
Rotation speed
Solution residual and monitor data
CFD-Post offers limited or no functionality in these areas when reading CFF files from CFX:
Mesh coordinate transformations
CFD-Post offers limited or no functionality in these areas when reading CFF files from Fluent:
Mesh (msh.h5) files (limited support)
Hanging nodes
Overset mesh
Particle tracks
Note that existing XML particle track files can be written by Fluent and read into CFD-Post.
Volume mesh data
Lattice Boltzmann: mesh or data
The same limitations that CFD-Post has with reading legacy files from Fluent, as described in Limitations with Ansys Fluent Files
The following topics are discussed:
Names read from CFF files are preserved as much as possible unless a non-native naming convention is used for variables. However, CFD-Post might change some characters in any name to meet the requirements of the expression language and CCL.
There is a user preference, Common Fluids Format > Name Convention, that controls the optional renaming of variables loaded from CFF files. For details, see Variables.
Fluent species names may not be consistent with those read from legacy cas/dat files. They are however, consistent with those seen in Fluent.
When reading Fluent files that lack the names of some periodic and symmetry boundaries, the names generated might differ from those generated when reading corresponding legacy files.
There is limited support for automatic Turbomachinery functionality.
You should always read transient data using the supplied
.flprj files. CFD-Post does not generate transient
sequences from a directory of CFF files.
CFD-Post reads and displays data as supplied by the solver, except when cell or face data is interpolated onto the vertices.
CFD-Post does not derive all the variables that are supported with legacy files. Some derived variables might show different values than those calculated when reading legacy files.
Some variable names might not be translated to CFD-Post names. There is limited support for variable name translation from some solvers.
Note: The following limitation applies to Solution files from Fluent:
Variable
Wall Adjacent Temperaturemight be incorrect.
Some functionality might be limited when compared to support for legacy results files. For details, refer to the documentation of the solver that writes the Common Fluids Format files.