6.3.6 I-deas Universal Files

You can import an I-deas Universal file into ANSYS FLUENT in three different ways.

• Generate an I-deas surface or volume mesh containing triangular, quadrilateral, tetrahedral, wedge and/or hexahedral elements. Import it into TGrid using the commands described in the TGrid User's Guide. Adhere to the restrictions described in Appendix B of the TGrid User's Guide. In TGrid, complete the mesh generation (if necessary) and follow the instructions in Section  6.3.3.

• Generate an I-deas volume mesh with linear triangular, quadrilateral, tetrahedral, wedge, or hexahedral elements. Import it directly using the File/Import/I-deas Universal... menu item, as described in Section  4.12.10.

• Generate an I-deas volume mesh with linear triangular, quadrilateral, tetrahedral, wedge, or hexahedral elements. Use the fe2ram filter to convert the Universal file to the format used by ANSYS FLUENT. To convert an input file in I-deas Universal format to an output file in ANSYS FLUENT format, follow the instructions below in Section  6.3.11. After the output file is written, read it into ANSYS FLUENT using the File/Read/Mesh... menu item, as described in Section  4.2.

Recognized I-deas Datasets

The following Universal file datasets are recognized by the ANSYS FLUENT mesh import utility:

• Node Coordinates dataset number 15, 781, 2411

• Elements dataset number 71, 780, 2412

• Permanent Groups dataset number 752, 2417, 2429, 2430, 2432, 2435

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

Note:   The mesh area or mesh volume datasets are not recognized. This implies that writing multiple mesh areas/volumes to a single Universal file may confuse ANSYS FLUENT.

Grouping Nodes to Create Face Zones

Nodes are grouped in I-deas using the Group command to create boundary face zones. In ANSYS FLUENT, boundary conditions are applied to each zone. Faces that contain the nodes in a group are gathered into 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--i.e., every curve or mesh area will be a different zone in ANSYS FLUENT. You may also create the groups manually, generating groups consisting of all nodes related to a given curve (2D) or mesh area (3D).

Grouping Elements to Create Cell Zones

Elements in I-deas are grouped using the Group 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.

Deleting Duplicate Nodes

I-deas may generate duplicate or coincident nodes in the process of creating elements. These nodes must be removed in I-deas before writing the universal file for import into ANSYS FLUENT.