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.
The following Universal file datasets are recognized by the grid filter:
dataset number 15, 781, 2411
dataset number 780 or 2412
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.
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.
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).
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.
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.