Specifying Surface Body Thickness

The thickness of surface bodies can be prescribed in several ways:

  1. A uniform thickness over the entire body which can be defined inside Mechanical or imported from a CAD system. Thicknesses imported from CAD can be overridden by the Thickness Mode

  2. A constant or spatially varying thickness applied to a selection of surfaces or bodies.

  3. Thickness values imported from an upstream system.

  4. Layer information can be specified using a Layered Section, or imported through an Imported Plies.

See Faces With Multiple Thicknesses and Layers Specified for information on how Mechanical resolves conflicts when multiple thickness specifications are applied to the same geometry.

To specify the thickness of an entire surface body:

Highlight the surface Body object and, in the Details view, enter a value in the Thickness field. A value greater than 0 must be present in this field.

To specify the thickness of selected faces on a surface body:

  1. Highlight the Geometry folder in the tree and insert a Thickness object from the Geometry toolbar or choose Insert> Thickness (right-click and choose from context menu).


    Note:  The Thickness object overwrites any element that is scoped to the selected surfaces that has thickness greater than 0 defined in the Details view of the surface Body object (See above).


  2. Apply scoping to selected faces on surface bodies.

  3. Set the desired shell offset.

  4. Define the thickness as a constant (default), with a table, or with a function:

    1. To define the thickness as a constant, enter the value in the Thickness field in the Details view.

    2. To define the thickness with a table:

      1. Click the Thickness field in the Details view, then click Tabular from the flyout menu.

      2. Set the Independent Variable in the Details view to X, Y, or Z.

      3. Choose a Coordinate System. The Global Coordinate System (Cartesian) is the default.

      4. Enter data in the Tabular Data window. The Graph window displays the variation of the thickness.

    3. To define the thickness with a function:

      1. Click the Thickness field in the Details view, then click Function from the flyout menu.

      2. Enter the function in the Thickness field. (Example: 45+10*x/591)

      3. Adjust properties in the Graph Controls category as needed:

        • Number of Segments - The function is graphed with a default value of 200 line segments. You can change this value to better visualize the function.

        • Range Minimum - The minimum range of the graph.

        • Range Maximum - The maximum range of the graph.


Note:
  • Surface body thicknesses must be greater than zero. Failures will be detected by the solver.

  • When importing surfaces bodies from DesignModeler, the associated thickness is automatically included with the import. See Importing Surface Body Thickness for details.

  • For the following, the nominal thickness of the body is used as opposed to the thickness controlled by the Thickness objects being added (Thickness, Layered Thickness, Imported Layered Thickness):

    • Geometry: the read-only physical properties, Volume, Mass, Centroid, and Moment of Inertia provided under the Details view Properties category of the Geometry object, Part object, and the Body object. The properties based on any variable thickness are correctly calculated in the solver and can be verified through miscellaneous record results for Mechanical APDL based solutions.

    • Meshing: during the meshing process, auto-detection based on surface body thickness, automatic pinch controls, surface body thickness used as mesh merging tolerance.

    • Solution: Heuristics used in beam properties for spot welds as well as moments applied to vertices.

  • Thickness objects are not supported for rigid bodies.

  • Variable thickness is displayed only for mesh and result displays. Location probes, Path scoped results, and Surface scoped results do not display nor account for variable thickness. They assume constant thickness.

  • If multiple Thickness objects are applied to the same face, only those properties related to the last defined object will be sent to the solver, regardless of whether the object was defined in DesignModeler or in Mechanical. See Faces With Multiple Thicknesses and Layers Specified for details.


You can import thicknesses from an upstream system. Basic setup steps are given below. You can find more information on mapping data in the Mechanical application in the appendix (Appendix B: Data Transfer Mapping and Validation).


Note:  Thickness import is supported for 3D shell bodies or planar 2D bodies using Plane Stress. The Mechanical APDL Solver for 3D shell bodies will use the nodal thicknesses directly via the SECFUNCTION command. For the Explicit Solver or MAPDL solver for 2D bodies, the element's nodal thicknesses are converted to an average element thickness.


To import thicknesses from an upstream system:

  1. In the project schematic, create a link between the Solution cell of a system and the Model cell of an upstream system.

  2. Attach geometry to the analysis system, and then double-click Model to open the Mechanical window. An Imported Thickness folder is added under the Geometry folder and an imported thickness is added to the Imported Thickness folder, by default.

  3. Select the appropriate options in the Details view.

  4. Select Imported Thickness and select Import Thickness from the context menu.


Release 18.2 - © ANSYS, Inc. All rights reserved.