The Remeshing tab allows you to introduce
one or more remeshing definitions within the configuration being edited.
To create a remeshing definition, click New 
. For additional details, see Remeshing Guide in the CFX Reference Guide.
Each remeshing definition requires that you:
Select either the User Defined or ICEM CFD Replay value for the Option setting. Additional settings, which depend on the option selected, are described in the sections User Defined Remeshing and Ansys ICEM CFD Replay Remeshing, presented below.
Select one or more activation condition(s) to be used to activate the remeshing object during the configuration’s execution. This selection is made from a list of the solver Interrupt Control conditions (for details, see Interrupt Control) that were defined for the Flow Analysis specified in the General Settings tab.
Select the mesh Location that will be replaced by remeshing. This selection is made from a list of the 3D mesh regions that are used in the Flow Analysis specified in the General Settings tab.
Each remeshing definition also allows you to specify a comma separated list of Mesh Reload Options that control how the new mesh replaces the previous one. The new mesh could, for example, be reloaded as a .gtm file using [mm] length units and all relevant mesh transformations by specifying:
Mesh Reload Options = "replacetype=GTM,replaceunits=mm,notransform=false"
These and other options are summarized in the table below.
Table 38.1: Reload Options
Reload Option | Description and Values |
|---|---|
notransform | True (default) ensures mesh transformations are not performed on mesh reload.
|
replacetype | Type of replacement mesh file.
|
replacegenargs | Generic mesh import options (as space separated list):
|
replacespecargs | Space-separated list of type-specific import arguments, as discussed in Supported Mesh File Types. |
replaceunits | Length units of the replacement mesh.
|
Full control over how the replacement mesh is generated is provided by the User Defined remeshing option. When this option is used, a user-defined command is required to gather all input data needed for remeshing and for create the replacement mesh file. The CFX-Solver, however, automatically executes the following tasks:
Import the new mesh into the problem definition
Interpolate solution data from the previous mesh onto the new mesh
Repartition the new mesh if a parallel run mode is used
Restart the equation solution process.
In addition to the required and optional general settings described above, the User Defined option requires specification of:
An External Command that is responsible for generating a replacement mesh file
The name of the Replacement File.
The External Command is submitted to the
operating system for execution. This may be a command to start a mesh
(re)generation executable directly with certain inputs, or a shell
script that executes several commands. It is important to note that
this command is submitted from the current run directory (for example case_001.dir), so care is required when using relative
paths to files during remeshing.
Useful inputs to the remeshing process may be extracted from
the most recently generated CFX-Solver Results file. For details, see Remeshing Guide in the CFX Reference Guide. This file is located in the run directory, and is simply
called res (no prefix or suffix) at the time
of submitting the External Command to the operating
system.
For additional details, see User Defined Remeshing in the CFX Reference Guide.
Remeshing using the Ansys ICEM CFD mesh generator is highly automated when the ICEM CFD Replay remeshing option is used. This is accomplished by combining settings made in the Flow Analysis (specified on the configuration’s General Settings tab) with a batch run of the Ansys ICEM CFD mesh generator using replay (session) files.
When this option is used the CFX-Solver automatically executes the following tasks:
Compile a comprehensive remeshing replay file from a combination of provided and user-specified replay files
Execute the Ansys ICEM CFD mesh generator in batch mode, using the remeshing replay file
Import the new mesh into the problem definition
Interpolate solution data from the previous mesh onto the new mesh
Repartition the new mesh if a parallel run mode is used
Restart the equation solution process.
In addition to the required and optional general settings described above, the ICEM CFD Replay option requires specification of:
An Ansys ICEM CFD Geometry File (with a tin extension) that contains the reference geometry
A Mesh Replay File (with an
rplextension) that contains a recording of the steps (that is, the commands) used to generate the mesh in the Ansys ICEM CFD application.
Additional, optional settings include:
ICEM CFD Geometry Control definitions
ICEM CFD Mesh Control definitions
Scalar Parameter definitions.
For additional details, see ICEM CFD Replay Remeshing in the CFX Reference Guide.
Option settings for ICEM CFD Geometry Control other than None are used to modify the reference geometry contained in the ICEM CFD Geometry File according to the mesh motion specifications defined in the CFX case setup. If the geometry control option is set to Automatic, then one or more ICEM CFD Part Map definitions may be defined. Each definition provides a mapping between:
An ICEM CFD Parts List, which is a list of parts (or families) defined in the referenced Geometry File
The translation of the centroid of a Boundary defined in the Flow Analysis.
These definitions are applied, in conjunction with
the default geometry control replay file (icemcfd_GeomCtrl.rpl contained the <CFXROOT>/etc/Remeshing
Options settings for ICEM CFD
Mesh Control other than None are used
to set values of some pre-defined parameters used by Ansys ICEM CFD during
remeshing. If the mesh control option is set to Automatic, then one or more ICEM CFD Part Parameter definitions
may be defined. Each definition provides a mapping for an ICEM CFD Parameter that governs mesh attributes like the
maximum element size (emax) or the maximum element
height (ehgt), between:
An ICEM CFD Parts List, which is a list of parts (or families) defined in the referenced Geometry File
A Monitor Point defined in the Flow Analysis.
These definitions are applied in conjunction with the
default mesh control replay file (icemcfd_MeshCtrl.rpl contained the <CFXROOT>/etc/Remeshing
Scalar Parameter definitions are used to set values of additional pre- or user-defined parameters referenced in any of the replay files used by Ansys ICEM CFD during remeshing. Each definition provides a mapping between a scalar parameter used during remeshing (with the same name as the Scalar Parameter definition) and a Monitor Point defined in the Flow Analysis.
The parameters listed in the table below are used in the default geometry control replay file, and become relevant if a Scalar Parameter definition is created with the same name.
Table 38.2: Scalar Parameters
Scalar Parameter | Description |
|---|---|
ICEM CFD Geometry Scale | The specified scale is used to address length unit differences between the geometry contained in the specified Ansys ICEM CFD Geometry File and the mesh contained in the CFX-Solver Input file. For example, if the length unit is [mm] in the Ansys ICEM CFD geometry and [m] in the CFX-Solver InputCFX-Solver Input file, then the geometry scale should be set to 0.001. |
OFFSET X OFFSET Y OFFSET Z | The specified offset values are added
to the centroid displacements (see the discussion on ICEM
CFD Geometry Control presented above) that are applied
for the part (or family) named |