The user interface commands related to the File menu (such as reading files, importing files) and other Select File dialog boxes do not work for the dual process
build. You need to use the TUI commands instead (for example, /file/read-mesh).
The host cannot be detached and reattached; once the connection is broken the data is lost. You need to save the data if the machine must be shut down in between.
All graphics information will be sent over the network, so initially it could take a long time to assemble graphical information (especially if the host and remote server are across continents) but after that the graphics manipulation is fast.
append-meshenables you to append the mesh files. This command is available only after a mesh file has been read in.
Append Rules:
If zone names and IDs are duplicated, they will be modified and the changes will be reported in the console.
Domain information will be retained during the file append operation. If domain names are duplicated, they will be modified and the changes will be reported in the console.
Refinement region information will be retained during the file append operation. If region names are duplicated, they will be modified and the changes will be reported in the console.
You can append files comprising only edge zones (without face zones).
Edge-face zone associations will be retained during the file append operation.
Zone-specific prism parameter information will be retained during the file append operation.
append-meshes-by-tmergeenables you to append the mesh files using the tmerge utility. This command is available only after a mesh file has been read in.
confirm-overwrite?controls whether attempts to overwrite existing files require confirmation.
If you do not want ANSYS Fluent to ask
you for confirmation before it overwrites existing files, you can
enter the file/confirm-overwrite? text command
and answer no.
file-formatenables/disables the writing of binary files.
filter-listlists the names of the converters that are used to change foreign mesh (while importing mesh files from third-party packages) files.
filter-optionsenables you to change the extension (such as .cas, .msh, .neu) and arguments used with a specified filter.
For example, if you saved the PATRAN files with a .NEU extension instead of .neu, you can substitute
or add .NEU to the extension list. For some
filters, one of the arguments will be the dimensionality of the grid.
When you use the filter-options command
for such a filter, you will see a default dimensionality argument
of -d a. The dimension will automatically
be determined, so you need not substitute 2 or 3 for a.
import/enables you to import mesh information generated by some CAD packages (ANSYS, I-deas, NASTRAN, PATRAN, and HYPERMESH), as well as mesh information in the CGNS (CFD general notation system) format.
These files are imported using the associated text commands listed here:
ansys-surf-meshenables you to read a ANSYS surface mesh file.
ansys-vol-meshenables you to read a ANSYS volume mesh file.
cadenables you to import CAD files based on the options set.
To import a single file (default), specify the file path and set up options for extracting features, importing curvature data from CAD, and the length unit.
To import multiple files, specify the directory path and pattern, and set up options for appending the files, extracting features, importing curvature data from CAD and the length unit.
cad-geometryenables you to import CAD files based on the options set.
To import a single file (default), specify the file path. Set up options for the length unit, tessellation method, and sizing parameters based on the tessellation method.
To import multiple files, specify the directory path and pattern. Set up options for appending the files, the length unit, tessellation method, and sizing parameters based on the tessellation method.
cad-options/contains additional options for importing CAD files.
continue-on-error?enables you to continue the import of the CAD file(s), despite errors or problems creating the faceting on certain surfaces, or other issues. This option is disabled by default.
create-cad-assemblies?enables creating the CAD Assemblies tree on CAD import. The CAD Assemblies tree represents the CAD tree as it is presented in the CAD package in which it was created. All sub-assembly levels from the CAD are maintained on import in Fluent Meshing.
For commands specific to the CAD assemblies, refer to cad-assemblies/
derive-zone-name-from-object-scope?enables zones without Named Selections to inherit the object name on import. This option is disabled by default.
double-connected-face-labeladds the specified label to the name of double-connected face zones (face zones shared by two bodies).
enclosure-symm-processing?enables processing of enclosure and symmetry named selections during import. This option is disabled by default. This option is applicable only to ANSYS DesignModeler (*.agdb) files.
extract-features?enables feature extraction from the CAD model on import. You can choose to disable this, if desired. Specify an appropriate value for feature angle. The default value is 40.
import-body-names?enables import of Body names from the CAD files. This option is enabled by default.
Note: Any renaming of Body names in ANSYS Mechanical/ANSYS Meshing prior to the export of the mechdat/meshdat files is ignored during import. Only original Body names will be imported.
import-curvature-data-from-CAD?enables importing of the curvature data from the nodes of the CAD facets. You can choose to disable this, if desired.
import-part-names?enables import of Part names from the CAD file(s). This option is enabled by default.
Note: Any renaming of Part names in ANSYS Mechanical/ANSYS Meshing prior to the export of the mechdat/meshdat files is ignored during import. Only original Part names will be imported.
merge-nodes?enables the merging of geometry object nodes during CAD import. This option is enabled by default.
Note: This option can be optionally enabled/disabled only when geometry objects are imported using the CAD Faceting option for CAD import. Mesh object nodes will always be merged when the CFD Surface Mesh is selected for CAD import.
modify-all-duplicate-names?enables you to modify all duplicate object/zone names by adding incremental integers as suffix. This option is disabled by default.
For example: The CAD file contains multiple parts (or bodies) named heatshield.
With the option disabled (default), the imported zones will be named heatshield, heatshield.1, heatshield.2, etc.
With the option enabled, the imported zones will be named heatshield.1, heatshield.2, heatshield.3, etc.
name-separator-characterallows you to specify the character used between name fields. Default is ':'.
named-selectionsenables you to import Named Selections from the CAD file(s), including Named Selections from ANSYS DesignModeler,
publications from CATIA, and so on. You can additionally choose
to ignore import of certain Named Selections based on the pattern
specified (for example, Layer* to ignore
layer Named Selections from CATIA), or by specifying multiple
wild cards (for example, ^(Color|Layer|Material).* to remove color, layer, and material Named Selections from CATIA).
Named Selections defined in ANSYS Meshing cannot be imported.
If Named Selections is enabled, then Face named selections will be imported as face zone labels.
object-typeenables the setting of object type on import. The
options available are auto, geometry, and mesh. The default setting is auto based on the tessellation method selected: geometry
objects will be created when the cad-faceting method is used, while mesh objects will be created when the cfd-surface-mesh method is used.
one-face-zone-perenables you to create one face zone per body/face/object to be imported.
one-object-perenables you to create one object per body/part/file/selection to be imported.
Note: For ANSYS ICEM CFD files (*.tin), set the object granularity to one object per selection.
read-all-cad-in-subdirectories?when enabled, all files in the specified directory as well as in its subdirectories will be imported. This option is disabled by default.
save-PMDB?saves a PMDB (*.pmdb) file in the directory containing the CAD files imported. You can use this file to import the same CAD file(s) again with different options set, for a quicker import than the full import. This option is disabled by default.
Note: Some options will not be available any more once the model
is imported from a PMDB file (for example, enclosure-symm-processing?), since they are processed before the PMDB file is created.
separate-features-by-type?enables separation of feature edges based on angle, connectivity, and named selections on import. Edge zone names will have suitable suffixes depending on separation criteria, order of zones, existing zone names and other import options selected.
single-connected-edge-labeladds the specified label to the name of single-connected edge zones (edge zones referenced by a single face).
strip-file-name-extension-from-naming?removes the extension of the CAD files from the object/face zone names on import. This option is disabled by default.
strip-path-prefix-from-names?enables you to remove the path prefix from the object/face zone names on import. The default
setting is auto which removes the path prefix from object/face zone names
when the object creation granularity is set to one object per file. You can also explicitly select
yes or no.
tessellationenables you to control the tessellation (faceting)
during file import. You can select either cad-faceting or cfd-surface-mesh.
CAD faceting enables you to control the tessellation based on the CAD faceting tolerance and maximum facet size specified.
CFD Surface Mesh enables you to use a size field file, (Use size field file?). If you enter yes, specify the size field file to be read. If you do not want to use
a size field file, you can obtain conformal faceting based on the
underlying curve and surface curvature (using the minimum and maximum
facet sizes, and the facet curvature normal angle specified) and edge
proximity (using the cells per gap specified). You can also save a
size field in a file (size field is computed based on the specified
parameters; that is, Min Size, Max
Size, Curvature Normal Angle, Cells Per Gap).
use-collection-names?enables you to use the Named Selections for the object/zone
names on import. Select auto, no, or yes. The default selection
is auto where the Named Selection will be
used as the object/zone name, except when the object creation granularity
is set to one object per file.
use-component-names?enables you to add the component (part or assembly) names to the
object/zone names on import. Select auto,
no, or yes. The default selection is
auto where the component name will be added to the object/zone
name.
use-part-names?enables you to choose whether to add the part names from the CAD file to the object and zone
names on import. The default setting is auto which adds the part names to
both object and zone names when object creation granularity is set to body.
When the object creation granularity is set to part or
file, the part names are not added to the zone names, face zone labels, or the
region names, by default. You can also explicitly select yes or
no.
use-part-or-body-names-as suffix-to-named-selections?enables you to modify zone names by using part or body names as suffixes to the Named Selections spanning multiple parts/bodies. This option is enabled by default.
For example: The CAD file contains a Named Selection effusion with part (or body) names id_liner and od_liner.
With the option enabled (default), the imported zones will be named effusion:id_liner and effusion:od_liner.
With the option disabled, the imported zones will be named effusion.1 and effusion.2.
cgns-surf-meshenables you to read a CGNS surface mesh file.
cgns-vol-meshenables you to read a CGNS volume mesh file.
fidap-surf-meshenables you to read a FIDAP surface mesh file.
fidap-vol-meshenables you to read a FIDAP volume mesh file.
fl-uns2-meshenables you to read a Fluent UNS V2 case file.
fluent-2d-meshenables you to read a 2D mesh into the 3D version.
gambit-surf-meshenables you to read a GAMBIT surface mesh file.
gambit-vol-meshenables you to read a GAMBIT volume mesh file.
hypermesh-surf-meshenables you to read a HYPERMESH surface mesh file.
hypermesh-vol-meshenables you to read a HYPERMESH volume mesh file.
ideas-surf-meshenables you to read an I-deas surface mesh file.
ideas-vol-meshenables you to read an I-deas volume mesh file.
nastran-surf-meshenables you to read a NASTRAN surface mesh file.
nastran-vol-meshenables you to read a NASTRAN volume mesh file.
patran-surf-meshenables you to read a PATRAN surface mesh file.
patran-vol-meshenables you to read a PATRAN volume mesh file.
load-act-toolloads the ANSYS ACT tool.
read-boundary-meshenables you to read a boundary mesh. If the boundary mesh is contained in two or more separate files, you can read them in together and assemble the complete boundary mesh.
This option is also convenient if you want to reuse the boundary mesh from a file containing a large volume mesh.
Note: The naming of face zones can be controlled by Named Selections defined in ANSYS Workbench. For details on exporting faceted geometry from ANSYS Workbench, refer to the ANSYS Workbench Help.
read-caseenables you to read the mesh contained in a case file.
Note: Cell hierarchy in case files adapted in the solution mode will be lost when they are read in the meshing mode.
Case files containing polyhedral cells can also be read in the meshing mode of Fluent. You can display the polyhedral mesh, perform certain mesh manipulation operations, check the mesh quality, and so on.
read-domainsenables you to read domain files.
Each mesh file written by Fluent has a domain section. A domain file is the domain section of the mesh file and is written as a separate file. It contains a list of node, face, and cell zone IDs that make up each domain in the mesh.
If a domain that is being read already exists in the mesh, a warning message is displayed. Fluent verifies if the zones defining the domains exist in the mesh. If not, it will display a warning message.
read-journalenables you to read a journal file into the program.
The read-journal command always loads
the file in the main (that is, top-level) menu, regardless of where
you are in the menu hierarchy when you invoke it.
read-meshenables you to read a mesh file. You can also use this command to read a Fluent mesh file created with GAMBIT, or to read the mesh available in a Fluent case file.
Note: Reading a case file as a mesh file will result in loss of boundary condition data as the mesh file does not contain any information on boundary conditions.
Case files containing polyhedral cells can also be read in the meshing mode of Fluent. You can display the polyhedral mesh, perform certain mesh manipulation operations, check the mesh quality, and so on.
Important: You cannot read meshes from solvers that have been adapted using hanging nodes. To read one of these meshes in the meshing mode in Fluent, coarsen the mesh within the solver until you have recovered the original unadapted grid.
Note: The naming of face zones can be controlled by Named Selections defined in ANSYS Workbench. For details on exporting faceted geometry from ANSYS Workbench, refer to the ANSYS Workbench Help.
read-meshes-by-tmergeuses the tmerge utility to read the mesh contained in two or more separate files. It enables you to read the mesh files together and helps assemble the complete mesh.
read-multi-bound-meshenables you to read multiple boundary mesh files into the meshing mode.
read-multiple-meshenables you to read in two or more files together and have the complete mesh assembled for you, if the mesh files are contained in two or more separate files.
For example, if you are going to create a hybrid mesh by reading in a triangular boundary mesh and a volume mesh consisting of hexahedral cells, you can read both files at the same time using this command.
read-optionsenables you to set the following options for reading mesh files:
Enforce mesh topology: This option is disabled by default. Enabling this option will orient the face zones consistently when the mesh file is read. If necessary, the zones being read will be separated, such that each boundary face zone has at most two cell zones as neighbors, one on either side. Also, internal face zones are inserted between neighboring cell zones that are connected by interior faces.
Check read data: This option enables additional checks
for the validity of the mesh. Enabling this option will check the
mesh topology during file read. In case incorrect mesh topology is
encountered, warning messages will be displayed and the erroneous
entities will be deleted. Note that in case of mesh topology errors,
no automatic mesh repair is done, and that parts of the mesh may be
non-conformal, contain voids, or be erroneous in other ways. The purpose
of the check-read-data option is to enable
access to corrupt files. This option is disabled by default with the
assumption that correct data will be read, and to shorten file read
times.
read-size-fieldenables you to read in a size field file.
Note: If you read a size-field file after scaling the model, ensure that the size-field file is appropriate for the scaled model (size-field vertices should match the scaled model).
set-tui-versionenables setting of the Fluent version for journal files. This is done automatically when a
journal file is created using the file/start-journal command. See Creating and Reading Journal Files for details.
show-configurationdisplays the current release and version information.
start-journalstarts recording all input and writes it to a file. The current Fluent version is automatically recorded in the journal file. Note that commands entered using paths from older versions of Fluent will be upgraded to their current path in the journal file. See Creating and Reading Journal Files in the ANSYS Fluent Meshing User's Guide.
To start the journaling process use the file/start-journal command,
and end it with the file/stop-journal command (or by exiting the program).
To read a journal file into the program, use the file/read-journal command.
Note: The read-journal command always loads the file in the main (that is,
top-level) menu, regardless of where you are in the menu hierarchy when you invoke it.
The standard period (.) alias is the same as the file/read-journal
definition and is defined by:
(alias ’. (lambda () (ti-read-journal)))
start-transcriptstarts recording input and output in a file.
A transcript file contains a complete record of all standard
input to and output from Fluent (usually all keyboard and user interface
input and all screen output).Start the transcription process with
the file/start-transcript command, and end
it with the file/stop- transcript command (or by exiting the program).
stop-journalstops recording input and closes the journal file.
stop-transcriptstops recording input and output, and closes the transcript file.
write-boundariesenables you to write the specified boundaries into a mesh file.
This is useful for large cases where you may want to mesh different parts of the mesh separately and then merge them together. This enables you to avoid frequent switching between domains for such cases. You can write out selected boundaries to a mesh file and then create the volume mesh for the part in a separate session. You can then read the saved mesh into the previous session and merge the part with the rest of the mesh.
write-caseenables you to write a case file that can be read by Fluent.
Note: You should delete dead zones in the mesh before writing the mesh or case file for Fluent.
write-domainsenables you to write all the mesh domains (except global) into a file that can be read.
write-meshenables you to write a mesh file.
Note: You should delete dead zones in the mesh before writing the mesh or case file for Fluent.
write-optionsenables you to set the enforce mesh topology option for writing mesh/case files.
This option is disabled by default; enabling this option will orient the face zones consistently when the mesh file is written. If necessary, the zones will be separated, such that each boundary face zone has at most two cell zones as neighbors, one on either side. Also, internal face zones will be inserted between neighboring cell zones that are connected by interior faces.
write-size-fieldenables you to write a size field file.