You can import CAD models using the CAD readers or associative geometry interfaces (via plug-ins). Refer to CAD Integration in the ANSYS Help for detailed CAD-related information.
Information about past, present, and future platform support is viewable via the ANSYS, Inc. Web site (Support > Platform Support), see ANSYS Platform Support.
Use the > > menu item to open the Import CAD Geometry dialog box, where you can set the basic options for importing CAD files.
By default, a single file will be imported. Disable Import Single File to import multiple files and specify the Directory and Pattern for the files to be imported.
Note: Ensure that the file path contains the appropriate platform-specific separators (for example, C:\Tutorials on Windows systems, Home/Tutorials on Linux systems).
The following special characters are supported in the file name:
| On Windows systems– + $ ^ ( ) [ ] { } @ # % _ - = , . ; ' ~ ` ! |
| On Linux systems– + $ ^ ( ) [ ] { } @ # % _ - = , . : ; ' > “ ~ ` ! |
Enable Append to append CAD model data to the existing model/mesh.
Note: The Append option is available only when a model/mesh has already been read.
You can select the length unit to scale the mesh on import; models created in other units will be scaled accordingly. The default selection is mm.
Important: The imported CAD models are scaled based on the length unit selected for the meshing mode session only. When the model is transferred to solution mode, the model units are reverted to the original CAD units. Refer to Scaling the Mesh in the Fluent User's Guide for details on scaling the mesh in solution mode.
The following Tessellation options are available:
If you select the CAD
Faceting option, you can choose to refine the CAD faceting. Enable
Refine Faceting and specify the
Tolerance for refinement and the Max
Size in the CAD Faceting Controls group box. The
default value for Tolerance is 0,
which implies no tessellation (faceting) refinement during import. The Max
Size enables you to specify a maximum facet size for the imported model
to avoid very large facets during the file import.
The Merge Nodes option in the CAD Options dialog box enables the merging of geometry object nodes during CAD import. This option is enabled by default when the CAD Faceting option is selected.
Use the default value of 0 for an initial
(diagnostic) import. You can then determine the minimum size you intend to use
for the mesh and import the file(s) again using a
Tolerance value 1/10th the intended minimum
size.
Due to merging of nodes on geometry objects, the sizing computed at the facet nodes may not represent the desired sizing. In this case, disable Merge Nodes in the CAD Options dialog box and re-import the geometry objects.
If you select the CFD Surface Mesh option, you need to specify the minimum and maximum facet sizes (Min Size, Max Size), and the Growth Rate.
Choose the type of Size Functions to be used for creating the surface mesh.
By default, a Curvature size function will be used for refining the surface mesh based on the underlying curve and surface curvature. Specify the Curvature Normal Angle to be used.
You can also use Proximity size functions for creating the surface mesh, based on the number of cells per gap specified. The proximity size functions can be scoped to edges, faces, or both faces and edges.
The Auto-Create Scoped Sizing enables you to create scoped sizing controls based on the defined parameters. This option is enabled by default.
You can also choose to save a size-field file based on the defined parameters ( Min Size, Max Size, Growth Rate, Curvature Normal Angle, and Cells Per Gap). The size-field will be read on CAD import.
Alternatively, you can use a previously saved size-field file to create the surface mesh by enabling Use Size Field File. Specify the Size Field File to be used.
Mesh object nodes will always be merged when the CFD Surface Mesh is selected for CAD import.
The Max Size value is limited to 1/10th the bounding box diagonal.
If you select a size-field file during CAD import, ensure that size-field file selected is appropriate for the length units selected.
Surfaces with failed surface meshes will be separated into distinct face zones and will have the "failed" identifier in the face zone name.
CFD Surface Mesh options are not supported for ANSYS ICEM CFD (*.tin) files.
Selecting CAD Faceting will result in Geometry Objects on import. Selecting CFD Surface Mesh will result in Mesh Objects on import.
The CAD Options dialog box contains additional options that can be set for importing CAD files. The following options are available:
You can choose to read all CAD files in the subdirectories of the selected directory.
Note: CAD files with only line bodies/wires (edge zones) cannot be imported.
You can save an intermediary PMDB (*.pmdb) file in the directory containing the CAD files imported. You can use this file to import the same CAD file(s) again with different options set, for a quicker import than the full import. A PMDB file will be saved per CAD file selected.
You can choose to process Named Selections from the CAD files, including Named Selections from ANSYS DesignModeler, publications from CATIA, and so on. Additional options to ignore import of Named Selections based on pattern or by wild card are available using the /file/import/cad-options/named-selections text command (see the Text Command List for details).
Note: Named Selections defined in ANSYS Meshing cannot be imported.
Important: In general, names from the CAD file are retained on import. Valid characters for object/zone names include all alphanumeric characters as well as the following special characters:
_ + - : .
All other characters, including spaces and slashes (/), are invalid. If an invalid character is specified, it is replaced by a hyphen (-) upon import.
A prefix zone will be added to the object name and face zone name if the body, part, file, or Named Selection name begins with a digit or a special character other than “_ :”. For example, importing a file .test.agdb with the option One object per file, will create an object named zone.test comprising the face zone zone.test.
A suffix -sheet will be added to the object name for surface bodies imported, except for surface bodies imported using the One Object per part option.
By default, the curvature data from the nodes of the CAD facets is imported. You can choose to disable this, if desired.
The Merge Nodes option enables the merging of geometry object nodes during CAD import.
This option is enabled by default when the CAD Faceting option is selected. However, due to merging of nodes on geometry objects, the sizing computed at the facet nodes may not represent the desired sizing. In this case, disable Merge Nodes and re-import the geometry objects.
Note: Mesh object nodes will always be merged when the CFD Surface Mesh is selected for CAD import.
By default, features will be extracted from the CAD model on import. You can choose to disable this, if desired.
Specify an appropriate value for Feature Angle. The default value is 40.
The Object Creation options enable you to set up object and zone granularity on import.
Enable Create CAD Assemblies to create the CAD Assemblies tree on CAD import. It represents the CAD tree as it is presented in the CAD package in which it was created. All sub-assembly levels from the CAD are maintained on import in Fluent Meshing. See CAD Assemblies for details.
You can specify CAD object and zone granularity using the options in the drop-down lists in the Object Creation group box. You can choose to create one CAD object per body (default), part, CAD file or selection imported. Similarly, you can choose to create one CAD zone per body (default), face, or object imported.
You can specify object and zone granularity using the options in the drop-down lists in the Object Creation group box. You can choose to create one object per body (default), part, CAD file or selection imported. Similarly, you can choose to create one face zone per body (default), face, or object imported.
Note: For ANSYS ICEM CFD files (*.tin), set the object granularity to one object per selection.
Important: When importing multi-body parts, it is recommended that the Object Creation option be set to one object per part or one object per file. In this case, by default, the part names from the CAD file will not be included in the zone names or added as a prefix to the face zone labels or region names.
Also, the Tessellation option should be set to CFD Surface Mesh to retain the same topology as in the CAD model.
By definition, objects do not share face and/or edge zones. If the Object Creation option is set to one object per body or one object per selection, common face/edge zones are duplicated on import to make the objects independent.
Additional import options are available via text commands, see the Text Command List for details.
You can continue to import the CAD files, despite errors or problems creating the faceting on certain surfaces, or other issues.
You can import part names and body names from the CAD files. You can also import enclosure and symmetry named selections from ANSYS DesignModeler (*.agdb) files.
You can separate feature edges based on angle, connectivity, and named selections on import. Edge zone names will have suitable suffixes depending on separation criteria, order of zones, existing zone names and other import options selected.
You can choose to add the component (assembly or part) name to the object/zone name. By default, the component name will be added to the object/zone name.
You can choose whether to add the part names from the CAD file to the object and
zone names on import. The default setting is auto which adds
the part names to both object and zone names when object creation granularity is set to
body. When the object creation granularity is set to
part or file, the part names are not added
to the zone names, face zone labels, or the region names, by default. You can also
explicitly select yes or no.
For zones without Named Selections, you can choose to inherit the object name on import. This option is disabled by default.
When importing Named Selections, the Named Selection will be used as the object/zone name by default, according the object creation granularity.
You can also choose to modify zone names by using part or body names as suffixes to the Named Selections spanning multiple parts/bodies. This option is enabled by default.
By default, Named Selections are not considered when the object creation granularity is set to one object per file. This behavior can be modified with the use-collection-names? text command.
You can also import the Named Selections as face zone labels when the CFD Surface Mesh option is selected for Tessellation.
You can also add labels to edges connected to a single face, edges connected to multiple faces, faces shared by bodies (double connected faces).
You can choose to remove the extension of the CAD files from the object/face zone names on import. This option is disabled by default.
You can choose to remove the path prefix from the object/face zone names on import.
The default setting is auto which removes the path prefix from
object/face zone names when the object creation granularity is set to one object per
file. You can also explicitly select yes or
no.
You can also choose to modify all duplicate object/zone names by adding incremental integers as suffix. This option is disabled by default.
Note:
Compressed CAD files (for example, *.stl.zip, *.stl.gz, *.stl.bz2) cannot be imported.
Filenames with DOS style 8.3 path (shorter path) cannot be imported. Ensure that you give the path name in full while importing the CAD files.
Virtual topology, suppressed parts/bodies, renamed parts/bodies defined in ANSYS Mechanical/ANSYS Meshing will be ignored during CAD import.
To import ANSYS DesignModeler files saved with blade geometry created using ANSYS BladeModeler (plug-in for ANSYS DesignModeler), ensure that the Geometry license preference is set to ANSYS BladeModeler as follows:
Select in the ANSYS Workbench menu.
Click the Geometry tab in the License Preferences dialog box.
If ANSYS BladeModeler is not the first license listed, then select it and click as required to move it to the top of the list.
When using the CATIA V5 Reader on Linux systems, body hierarchy information will not be available. Only the lowest “child” labels will appear in the tree. For more information, refer to CAD Integration in the ANSYS Help.
Tables of platform-specific supported CAD packages can be found at Linux or Windows.