A.3. Meshes from Third-Party CAD Packages

You can import grid files from third-party CAD packages by using the items in the File > Import menu. Alternatively, the fe2ram filter enables you to convert files created by several finite-element packages to the grid file format used by Fluent. You can convert surface or volume meshes from ANSYS, I-deas, NASTRAN, PATRAN, VRML files from VRML version 1.0, or other packages. ARIES files can be converted only if they are first saved as ANSYS Prep7 files, as described in ARIES Files.

If you choose to convert the file manually before reading it, enter the following command: 

utility fe2ram [dimension] read-format [merge] [zoning] [write-format] input-file output-file

The items in square brackets are optional.

  • dimension indicates the dimension of the dataset.

    • For a 3D grid, do not specify dimension as 3D is the default.

    • For a 2D grid, replace dimension by -d2.

    • For a surface mesh, replace dimension by -surface.

  • read-format indicates the format of the file you want to convert. Replace read-format as follows:

    • For an ANSYS file, use -tANSYS.

    • For an I-deas file, use -tIDEAS.

    • For a NASTRAN file, use -tNASTRAN.

    • For a PATRAN file, use -tPATRAN.

    For a list of conversion capabilities from other CAD packages, type utility fe2ram -cl -help.

  • merge indicates the grid tolerance. The default is 10-6 (1.0e-06). To set another tolerance value, replace merge by -mTOLERANCE, where TOLERANCE is an appropriate real number value. To reset the tolerance to the default value, replace merge by -m.

  • zoning indicates how zones were identified in the CAD package. Replace zoning as follows:

    • For a grid zoned by group, do not specify zoning as zoning by groups is the default.

    • For a grid that was zoned by property IDs, use -zID.

    • To ignore all zone groupings, use -zNONE.

  • write-format indicates the output format for the file you want to convert. Replace write-format as follows:

    • To write the grid for use in Fluent, do not specify write-format as this is the default.

    • To write the grid in FIDAP format, use -oFIDAP7.

  • input-file and output-file are the names of the original file and the file to which you want to write the converted grid information, respectively. Note that the output_file cannot be a CFF file (.msh.h5).

For example, to convert the 2D I-deas volume mesh file sample.unv to an output file called sample.msh, enter: 

utility fe2ram -d2 -tIDEAS sample.unv sample.msh

After the output file has been written, you can read it using File > Import in the meshing mode of Fluent. For volume meshes, the resulting output file can also be read into the solution mode of Fluent.

Important:  All boundary types are considered to be wall zones. You can set the appropriate boundary types in meshing mode or in solution mode.

Note:  The fe2ram utility supports VRML files from VRML version 1.0.

 

A.3.1. I-deas Universal Files

For I-deas surface meshes, the filter reads triangular and quadrilateral elements that define the boundaries of the domain and have been grouped within I-deas to create zones. For volume meshes, the filter reads a 2D or 3D mesh that has its boundary nodes or 2D boundary elements appropriately grouped to create boundary zones. Do not include nodes and boundary elements in the same group. All boundary zones will be considered wall zones; you can set the appropriate boundary types in the meshing mode or in the solution mode. See Meshes from Third-Party CAD Packages for further details.

 

A.3.1.1. Recognized I-deas Datasets

The following Universal file datasets are recognized by the grid filter:

Node Coordinates

dataset number 15, 781, 2411

Elements

dataset number 780 or 2412

Permanent Groups

dataset number 752, 2417, 2429, 2430, 2432, 2435

Because Fluent uses linear elements, you should use linear elements to generate the grid inside the mesh areas. If parabolic elements exist in the dataset, the filter ignores the mid side nodes. This assumption is valid if the edges of the element are near linear. However, if this is not the case, an incorrect topology may result from this assumption. For example, in regions of high curvature the parabolic element may look much different than the linear element.

For volume meshes, note that mesh area/mesh volume datasets are not recognized. This implies that writing multiple mesh areas/mesh volumes to a single Universal file may confuse fe2ram or Fluent.

 

A.3.1.2. Grouping Elements to Create Zones for a Surface Mesh

The Group command in I-deas is used to create the boundary zones needed by Fluent. All faces grouped together are listed together in the output as a single zone. In Fluent, boundary conditions are set on a per-zone basis.

One technique is to generate groups automatically based on mesh areas—that is, every mesh area will be a different zone. Although this method may generate a large number of zones, the zones can be merged in the meshing mode or in the solution mode of Fluent. Another technique is to create a group of elements related to a given mesh area manually. This enables you to select multiple mesh areas for one group.

 

A.3.1.3. Grouping Nodes to Create Zones for a Volume Mesh

The Group command is used in I-deas to create the boundary zones needed by Fluent. All nodes grouped together are listed together in the output as a single zone. It is important not to group nodes of internal faces with nodes of boundary faces.

One technique is to generate groups automatically based on curves or mesh areas—that is, every curve or mesh area will be a different zone in Fluent. Another technique is to create the groups manually, generating groups consisting of all nodes related to a given mesh area (3D).

 

A.3.1.4. Periodic Boundaries

In general, it is difficult to generate a valid grid with periodic boundaries in I-deas. However, a special feature exists in the meshing mode in Fluent that enables you to generate a grid in a domain with periodic boundaries. See Creating Periodic Boundaries for further details.

 

A.3.1.5. Deleting Duplicate Nodes

I-deas often generates duplicate nodes in the process of creating triangular elements. These must be removed by using either the remove coincident node command in I-deas or the Merge button in the Merge Boundary Nodes dialog box (or the /boundary/merge-duplicates text command). This node merging process is usually faster in the meshing mode in Fluent but more visual in I-deas.

 

A.3.2. PATRAN Neutral Files

For PATRAN surface meshes, the filter reads triangular and quadrilateral linear elements that define the boundaries of the domain and have been grouped by named component or identified by property IDs within PATRAN to create zones. For volume meshes, the filter reads a 2D or 3D mesh that has its boundary nodes grouped by named component to create boundary zones. All boundary zones will be considered wall zones; you can set the appropriate boundary types in the meshing mode or in the solution mode of Fluent. See Meshes from Third-Party CAD Packages for details.

 

A.3.2.1. Recognized PATRAN Datasets

The following Neutral file datasets are recognized by the grid filter:

Node Data

Packet Type 01

Element Data

Packet Type 02

Distributed Load Data

Packet Type 06

Node Temperature Data

Packet Type 10

Name Components

Packet Type 21

File Header

Packet Type 25

 

A.3.2.2. Grouping Elements to Create Zones

In PATRAN, named components are applied to the nodes to create groups of faces called zones. In Fluent, boundary conditions are applied to each zone. For example, all nodes on a curve or patch can be put in a Name Component.

For 2D volume meshes, an additional constraint is placed on the elements: existence in the Z=0 plane.

 

A.3.2.3. Periodic Boundaries

In general, it is difficult to generate a valid grid with periodic boundaries in PATRAN. However, a special feature exists in the meshing mode in Fluent that enables you to generate a grid in a domain with periodic boundaries. See Creating Periodic Boundaries for further details.

 

A.3.3. ANSYS Files

For ANSYS surface meshes, the filter reads triangular and quadrilateral linear elements that define the boundaries of the domain and have been grouped within ANSYS using node and element selection. For volume meshes, the filter reads a 2D or 3D mesh that has its boundary nodes grouped within ANSYS using node and element selection. All boundary zones will be considered wall zones; you can set the appropriate boundary types in the meshing mode or in the solution mode in Fluent. See Meshes from Third-Party CAD Packages for details.

 

A.3.3.1. Recognized Datasets

The following datasets are recognized by the grid filter:

NBLOCK

node block data

EBLOCK

element block data

CMBLOCK

element/node grouping

The elements must be STIF63 linear shell elements. In addition, if element data without an explicit element ID is used, the filter assumes sequential numbering of the elements when creating the zones.

 

A.3.3.2. Periodic Boundaries

In general, it is difficult to generate a valid grid with periodic boundaries in ANSYS. However, a special feature exists in the meshing mode in Fluent that enables you to generate a grid in a domain with periodic boundaries. See Creating Periodic Boundaries for further details.

 

A.3.4. ARIES Files

ARIES provides a filter or you may write a Prep7 file from ARIES and use the fe2ram filter with arguments for an ANSYS file. For more information on importing ANSYS files, see ANSYS Files.

In general, to write a Prep7 file within ARIES the following criteria must be met:

  • Name the part in the Geom module.

  • Create a material or read one from the mat_lib in the Material module. To create a material, you must supply density, Poisson’s ratio, and elastic modulus.

  • Generate face pressures for the surface in the Environment module. Later, when you write the Prep7 file, these will be transferred to the individual elements.

  • Generate at least one restraint in the Environment module.

  • Set the element type to be STIF63 (triangular shell elements) and specify some finite thickness.

  • Write the Prep7 file, making sure you let it automatically assign the pressure to the elements.

You can filter the Prep7 file by using the ARIES or Fluent filter, whichever you find most convenient.

 

A.3.5. NASTRAN Files

For NASTRAN surface meshes, the filter reads triangular and quadrilateral linear elements that define the boundaries of the solution domain. For volume meshes, the filter reads a 2D or 3D mesh. All boundary zones are considered wall zones; you can set the appropriate boundary types in the meshing mode or in the solution mode in Fluent. For details, see Meshes from Third-Party CAD Packages.

 

A.3.5.1. Recognized NASTRAN Bulk Data Entries

The following NASTRAN bulk entries are recognized by the grid filter:

GRID

single-precision node coordinates

GRID*

double-precision node coordinates

CBAR

line elements

CTETRA, CTRIA3

tetrahedral and triangular elements

CHEXA, CQUAD4, CPENTA

hexahedral, quadrilateral, and wedge elements

Because Fluent uses linear elements, you should use linear elements in the mesh-generation process. If parabolic elements exist in the dataset, the filter ignores the mid-side nodes. This assumption is valid if the edges of the element are near linear. However, if this is not the case, an incorrect topology may result from this assumption. For example, in regions of high curvature the parabolic element may look much different than the linear element.

 

A.3.5.2. Periodic Boundaries

In general, it is difficult to generate a valid grid with periodic boundaries in NASTRAN. However, a special feature exists in the meshing mode in Fluent that enables you to generate a grid in a domain with periodic boundaries. For details, see Creating Periodic Boundaries.

 

A.3.5.3. Deleting Duplicate Nodes

NASTRAN often generates duplicate nodes in the process of creating triangular elements. You must remove them by clicking Merge in the Merge Boundary Nodes dialog box (or by using the /boundary/merge-duplicates text command).