### 34.2.2. Remeshing Tab

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:

1. 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.

2. 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.

3. 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 34.1: Reload Options

Reload Option | Description and Values
--- | ---
notransform | True (default) ensures mesh transformations are not performed on mesh reload. `True` or `False`

replacetype

Type of replacement mesh file.

`ANSYS`: cdb and inp files

`CFX4`: geo files

`CFX5`: CFX 5.1 files

`CGNS`: cgns and cgn files

`GEM`: TfC files

`GTM`: gtm files

`GtmDirect`: def and res files

`GTM_DSDB`: ANSYS cmdb and dsdb files

`Def`: def files that are older than CFX 5.6 (or if duplicate node removal is required)

`Fluent`: cas and msh files

`Generic`: ICEM CFD mesh (cfx, cfx5, msh) files

`GRD`: CFX-TASCflow (grd) files

`IDEAS`: unv files

`MSC`: Patran out and neu files

`PDC`: GridPro files

replacegenargs | Generic mesh import options (as space separated list): `-g`: Ignore degenerate element errors `-n`: Do not do duplicate node removal `-T`: specify duplicate node removal tolerance (float). `-D`: Primitive naming strategy ; either `Standard Naming Strategy` or `Derived Naming Strategy`.
replacespecargs | Space-separated list of type-specific import arguments, as discussed in Supported Mesh File Types.
replaceunits | Length units of the replacement mesh. `micron`, `mm`, `cm`, `m`, `in`, `ft`

#### 34.2.2.1. User Defined Remeshing

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.

#### 34.2.2.2. ANSYS ICEM CFD Replay Remeshing

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 `rpl` extension) 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.

##### 34.2.2.2.1. ICEM CFD Geometry Control

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` directory), to modify the reference geometry prior to regenerating the mesh. If the geometry control option is set to User Defined Replay File, then a File Name is required and the specified file is used instead of the default geometry control replay file.

##### 34.2.2.2.2. ICEM CFD Mesh Control

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` directory), to modify the reference geometry prior to regenerating the mesh. If the mesh control option is set to User Defined Replay File, then a File Name is required and the specified file is used instead of the default mesh control replay file.

##### 34.2.2.2.3. Scalar Parameter

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 34.2: 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 `PartName` OFFSET Y `PartName` OFFSET Z `PartName` | 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 `PartName`. Note that the ICEM CFD Geometry Scale is also applied to the offset specified offset.

Release 18.2 - © ANSYS, Inc. All rights reserved.