Meshing Options on the Options Dialog Box

The options that appear in the right pane of the Options dialog box depend on which category is selected in the left pane:

  • When Meshing is selected in the left pane, these subcategories appear:

    • Meshing

    • Virtual Topology

    • Sizing

    • Quality

    • Inflation

  • When Export is selected in the left pane, these subcategories appear:

    • CGNS

    • Ansys Fluent

Meshing

  • Highlight Topology Being Meshed if Possible: Controls the default for highlighting of topologies during mesh processing. When Yes (default), the topology that is currently being processed by the mesher is highlighted in the Geometry window, which may help with troubleshooting. This highlighting is not supported for the Patch Independent Tetra or MultiZone mesh methods, or when assembly meshing is being used. Refer to Generating Mesh for details.

  • Allow Selective Meshing: Allows/disallows selective meshing. Choices are Yes and No. The default value is Yes. Refer to Selective Meshing for details.

  • Number of CPUs for Meshing Methods: Specifies the number of processors to be used by the meshing operation. There is no counterpart setting in the Details View. Specifying multiple processors will enhance the performance of the MultiZone Quad/Tri, Patch Independent Tetra, and MultiZone mesh methods. This option has no effect when other mesh methods are being used. You can specify a value from 0 to 256 or accept the default. The default is 0, which means the number of processors will be set automatically to the maximum number of available CPUs. The Number of CPUs option is applicable to shared memory parallel (SMP) meshing (multiple cores; not supported for clusters). Refer to Parallel Part Meshing.

  • Default Physics Preference: Sets the default option for the Physics Preference in the Details View of a Mesh object. Choices are Mechanical, Nonlinear Mechanical, Electromagnetics, CFD, Explicit, and Hydrodynamics.

  • Default Method: Sets the default Method setting in the Details View of a Method control object. This option only affects Method controls that are added manually. Choices are Automatic (Patch Conforming/Sweeping), Patch Independent, and Patch Conforming. When the geometry is attached, the default method of all options except Automatic will be scoped to all parts in the assembly. The Automatic option has no effect.

    Note:  Changing the Default Method changes the default mesh method for all future analyses, regardless of analysis type.

  • Use MultiZone for Sweepable Bodies: If set to On, the mesher uses the MultiZone method instead of General Sweeping for sweepable bodies. The default setting is Off. See MultiZone for Sweepable Bodies for more information.

  • Solid –Shell Weld- Shared Nodes: Generates weld between shell and solid bodies but the node connection between the weld and solid bodies are not conformal. Instead, bonded contact is created while solving when Solid –Shell Weld- Shared Nodes is No. When Solid –Shell Weld- Shared Nodes is Yes, creates conformal mesh without contacts between the shell and weld bodies.

  • Topology Checking: Sets the default value for the Topology Checking control. The default value is Yes.

  • Verbose Messages from Meshing: Controls the verbosity of messages returned to you. If set to On and you are meshing a subset of bodies, the message "These bodies are going to be meshed" appears, and you can click the right mouse button on the message to see the bodies. The default is Off. Regardless of the setting, when meshing completes and any bodies failed to mesh, the message "These bodies failed to be meshed" appears, and you can click the right mouse button to see them.

  • Number of CPUs for Parallel Part Meshing: Sets the default number of processors to be used for parallel part meshing. You can change this value in the Advanced group under the Details View. Using the default for specifying multiple processors will enhance meshing performance on geometries with multiple parts. For parallel part meshing, the default is set to Program Controlled or 0. This instructs the mesher to use all available CPU cores. The Default setting inherently limits 2 GB memory per CPU core. An explicit value can be specified between 0 and 256, where 0 is the default. Refer to Parallel Part Meshing for more details.

  • Show Only Non-Zero Mesh Element Statistics: Enables you to view the counts for all element types even the ones that do not exist in the mesh when set to No. The default value is Yes.

  • Redraw Graphics after Each Mesh Generation: Displays the graphics for every step in the Mesh Worksheet after completing the mesh generation for the respective step, when set to Yes. The default value is Yes. Redraw Graphics after Each Mesh Generation applicable only when Mesh Worksheet is created and active.

Virtual Topology

Merge Edges Bounding Manually Created Faces: Sets the default value for the Merge Face Edges setting in the Details View of a Virtual Topology object. Choices are Yes and No. The default value is Yes.

Sizing

  • Adaptive Resolution: Sets the resolution for mesh sizing when Use Adaptive Sizing is set to Yes. The default setting is Program Controlled. The range of values that can be set is 0 to 7, with the mesh resolution changing from coarse (0) to fine (7). See Resolution for more information.

  • Mechanical Min Size Factor (Default: 0.01): Sets your preference for the scale factor that will be used to calculate the default minimum size when the physics preference is Mechanical, Electromagnetics, or Explicit. The value that is specified here is multiplied by the global element size to determine the default minimum size.

  • CFD Min Size Factor (Default: 0.01): Sets your preference for the scale factor that will be used to calculate the default minimum size when the physics preference is CFD. The value that is specified here is multiplied by the global element size to determine the default minimum size.

  • Explicit Min Size Factor (Default: 0.5): Sets your preference for the scale factor that will be used to calculate the default minimum size when the physics preference is Explicit. The value that is specified here is multiplied by the global element size to determine the default minimum size.

  • Mechanical Defeature Size Factor (Default: 0.005): Sets your preference for the scale factor that will be used to calculate the default defeature size when the physics preference is Mechanical, Electromagnetics, or Explicit. The value that is specified here is multiplied by the global element size to determine the default defeature size.

  • CFD Defeature Size Factor (Default: 0.005): Sets your preference for the scale factor that will be used to calculate the default defeature size when the physics preference is CFD. The value that is specified here is multiplied by the global element size to determine the default defeature size.

  • Explicit Defeature Size Factor (Default: 0.1): Sets your preference for the scale factor that will be used to calculate the default defeature size when the physics preference is Explicit. The value that is specified here is multiplied by the global element size to determine the default defeature size.

  • Bounding Box Factor (Default: 0.05): Helps set the default Element size as follows: (Bounding Box Diagonal * Bounding Box Factor = Default Element size). This is only used when Use Adaptive Sizing is set to No and only solid parts are present in the model. Adaptive sizing uses its own default.

  • Surface Area Factor (Default: 0.125): Helps set the default Element size as follows: sqrt(Average Surface Area) * Surface Area Factor = Default Element Size). This is only used when Use Adaptive Sizing is set to No and sheet bodies are present in the model. Adaptive sizing uses its own default.

  • Explicit Particle Diameter Factor (Default: 0.5): Sets your preference for the scale factor that will be used to calculate the default Particle Diameter when the physics preference is Explicit. The value that is specified here is multiplied by the global Particle Diameter to determine the default Particle Diameter.

  • MultiZone Sweep Sizing Behavior: If set to Use Size Function, then any applied sizing controls (curvature and proximity refinement, and/or local sizing) are evaluated in all directions of the selected bodies. If set to Ignore Size Function, curvature and proximity refinement and/or local sizing along the sweep path are ignored and the spacing along the sweep path is determined either by the global sizes or local sizes that are explicitly set on edges along the sweep direction.

    You can also override the sizing by locally specifying hard edge sizes or using the Sweep Size Behavior control in the MultiZone method control to locally adjust the sizing for the bodies the control is scoped to. See MultiZone Method Control for more information.

  • Propagate Global to Local Settings: Enables you to use the global values for Capture Curvature and Capture Proximity as default local values when set to Yes. The default value is Yes.

Quality

  • Check Mesh Quality: Sets the default quality behavior with respect to how the mesher responds to error and warning limits. Choices are:

    • Default - With this setting, the behavior changes as appropriate when you change the setting of Physics Preference.

    • Yes, Errors - If the meshing algorithm cannot generate a mesh that passes all error limits, an error message is printed and meshing fails.

    • Yes, Errors and Warnings - If the meshing algorithm cannot generate a mesh that passes all error limits, an error message is printed and meshing fails. In addition, if the meshing algorithm cannot generate a mesh that passes all warning (target) limits, a warning message is printed.

    • No - Mesh quality checks are done at various stages of the meshing process (for example, after surface meshing prior to volume meshing). The No setting turns off most quality checks, but some minimal checking is still done. In addition, even with the No setting, the target quality metrics are still used to improve the mesh. The No setting is intended for troubleshooting and should be used with caution as it could lead to solver failures or incorrect solution results.

    • Mesh Quality Worksheet: Perform mesh checks after mesh completion based on user defined warning and error limits set in the Mesh Quality Worksheet.

  • Mechanical Error Limit: Sets the default error limit when Physics Preference is set to Mechanical. Choices are Standard Mechanical and Aggressive Mechanical.

  • Target Element Quality (0 = Program Default): Sets the default target element quality. When you modify this value, the value you enter becomes the new default for the Target Element Quality in the Details View. You can enter 0 on the Options panel to revert to the program default.

  • Target Skewness (0 = Program Default): Sets the default target skewness. When you modify this value, the value you enter becomes the new default for the Target Skewness in the Details View. You can enter 0 on the Options panel to revert to the program default. For a tetrahedral mesh, you should not set Target Skewness to a value < 0.8.

  • Target Jacobian Ratio (Corner Nodes) (0 = Program Default): Sets the default target Jacobian ratio. When you modify this value, the value you enter becomes the new default Target Jacobian Ratio (Corner Nodes) in the Details View. You can enter 0 on the Options panel to revert to the program default.

  • Target Aspect Ratio (Explicit) (0 = Program Default): Sets the default target explicit aspect ratio. When you modify this value, the value you enter becomes the new default for the Target Explicit Aspect Ratio in the Details View. You can enter 0 on the Options panel to revert to the program default.

Inflation

Inflation-related options that can be set on the Options dialog box include:

CGNS

  • File Format: Sets the file format to be used for CGNS Export operations. There is no counterpart setting in the Details View. Choices are:

    • ADF (default) - Exports the mesh in ADF (Advanced Data Format).

    • HDF5 - Exports the mesh in HDF5 (Hierarchical Data Format version 5).

  • CGNS Version: Sets the CGNS library version to be used for CGNS Export operations. There is no counterpart setting in the Details View. Choices are 4.3 (the default), 3.3, 3.2, 3.1, 3.0, 2.5, 2.4, 2.3, 2.2, and 2.1.

  • Export Unit: Defines the unit of measurement for the mesh when exported to CGNS. The default is Use Project Unit, which means the mesh is not scaled. If you change this to another value (centimeter, millimeter, micrometer, inch, or foot), the mesh is scaled according to the export unit you select.

Ansys Fluent

  • Format of Input File (*.msh): Sets the file format to be used for Fluent Mesh Export operations. There is no counterpart setting in the Details View. Choices are Binary (the default) and ASCII.

  • Auto Zone Type Assignment: When set to On (the default), zone types are automatically assigned, as described in Fluent Mesh Export. When set to Off, assigns all boundary zones as the default WALL, enabling you to assign your own zone type assignments for Fluent Mesh Export operations.