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 the meshing mode of Fluent using the commands described in the Fluent Meshing User’s Guide. Adhere to the restrictions described in Appendix B: Mesh File Format of the Fluent Meshing User’s Guide. In meshing mode, complete the mesh generation (if necessary); then you can switch to the solution mode of Fluent or read it into a new Fluent session as described in Fluent Meshing Mode Mesh Files.
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... ribbon tab item, as described in I-deas Universal Files.
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 Using the fe2ram Filter to Convert Files. After the output file
is written, read it into ANSYS Fluent using the File/Read/Mesh... ribbon tab item, as described in Reading Mesh Files.
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 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.
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—that is, 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).
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.