6.3.8 PATRAN Neutral Files

There are three different ways in which you can import a PATRAN Neutral file into ANSYS FLUENT.

• You can generate a PATRAN surface or volume mesh containing triangular, quadrilateral, tetrahedral, wedge, and/or hexahedral elements, and import it into TGrid using the commands described in the TGrid User's Guide and adhering to the restrictions described in Appendix B of the TGrid User's Guide. In TGrid, complete the mesh generation (if necessary) and then follow the instructions in Section  6.3.3.

• You can generate a PATRAN volume mesh with linear triangular, quadrilateral, tetrahedral, wedge, or hexahedral elements (grouping nodes with the same component-group name) and import it directly to ANSYS FLUENT by selecting the
  File/Import/PATRAN menu item, as described in Section  4.12.14.

• You can generate a PATRAN volume mesh with linear triangular, quadrilateral, tetrahedral, wedge, or hexahedral elements and then use the fe2ram filter to convert the Neutral file into the format used by ANSYS FLUENT. To convert an input file in PATRAN Neutral format to an output file in ANSYS FLUENT format, follow the instructions below in Section  6.3.11. After the output file has been written, you can read it into ANSYS FLUENT using the File/Read/Mesh... menu item, as described in Section  4.2.

After reading a triangular or tetrahedral PATRAN volume mesh using the latter methods perform smoothing and swapping (as described in Section  27.13) to improve its quality.

Recognized PATRAN Datasets

The following PATRAN Neutral file packet types are recognized by the ANSYS FLUENT mesh import utility:

• 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

For 2D volume meshes, the elements must exist in a constant $z$ plane.

Grouping Elements to Create Cell Zones

Elements are grouped in PATRAN using the Named Component command to create the multiple cell zones. All elements grouped together are placed in a single cell zone in ANSYS FLUENT. If the elements are not grouped, ANSYS FLUENT will place all the cells into a single zone.