Defining Shell Section Properties

You can apply a shell section to define a structure in which one dimension (the thickness) is significantly smaller than the other two dimensions. The stresses in the thickness direction must also be negligible.

This task shows you how to:

Before you begin: To compute the shell thickness from the support, the support must have a thin parts attribute applied to the underlying geometry or a midsurface defined. For more information about thin part attributes, see the Simulation Model Preparation Guide. For more information about midsurface definition, see the Generative Shape Design Guide.
See Also
About Shell Sections
Ordered Geometric Sets
In Other Guides
Materials and Section Properties
About the Material Palette Interface
Support Selection

Define Shell Sections with Uniform Thickness

You can define a shell section that has the same thickness everywhere.

  1. From the Properties section of the action bar, click Shell Section .
  2. Optional: Enter a descriptive Name.
  3. Select a geometry support.

    You apply a shell section to one or more surface geometries. They must be the same surface features that the model uses as the supports for the corresponding mesh part in the FEM representation. You can also use geometry from an ordered geometric set.

    Note: When you mesh an edge fillet whose geoemetry is in a geometry set, apply the shell section property to the mesh feature to assign the section property to the entire region and not just to the fillets.

    For axisymmetric models, you select a cross-section that becomes a surface when the axisymmetric body is rotated. For more information, see About Axisymmetric Simulations.

    Tip: You can also assign local shell sections using the tools in the context toolbar. Click to assign a shell property to a group of faces, or click to assign a shell property to multiple surfaces that you select using the propagation method.

    If the support you select already has a material assigned to it, the Material field displays the material that is applied to the support.
  4. Optional: If there is no material assignment or you want to override the existing material assignment, do the following:
    1. Click .
      The Material Palette appears.
    2. Search for the material you want to assign, and click it.
    3. Click OK to close the Material Palette.
    The Material field displays the newly applied material.
  5. Select a material Behavior that is used in the simulation.
  6. Set the Thickness definition to Specified.
  7. For non-axisymmetric models, choose Uniform from the Thickness list, and enter a value for the thickness throughout the entire shell.
  8. Optional: If the materials in your model exhibit directional properties, define their orientation as part of the shell section definition. For more information, see Defining Material Orientations for Shell Sections.

    A material orientation is applied automatically for axisymmetric models.

  9. Specify whether you want the app to integrate the shell section before the analysis or during the analysis. For more information, see Choosing When to Integrate Shell Sections.
  10. Specify how you want to define the transverse shear stiffness. For more information, see Specifying Transverse Shear Stiffness Directly for Shell Sections.
  11. Click OK.

Define Shell Sections with Varied Thickness Using Mapped Data

You can define a shell section that has different thicknesses at different points.

Before you begin: You must have your spatially mapped data prepared. The mapped data can specify different thickness values at various points on the shell geometry.
  1. From the Properties section of the action bar, click Shell Section .
  2. Optional: Enter a descriptive Name.
  3. Select a geometry support.

    You apply a shell section to one or more surface geometries. They must be the same surface features that the model uses as the supports for the corresponding mesh part in the FEM representation. You can also use geometry from an ordered geometric set.

    Note: When you mesh an edge fillet whose geoemetry is in a geometry set, apply the shell section property to the mesh feature to assign the section property to the entire region and not just to the fillets.

    For axisymmetric models, you select a cross-section that becomes a surface when the axisymmetric body is rotated. For more information, see About Axisymmetric Simulations.

    You can also assign local shell sections using the tools in the context toolbar. Click to assign a shell property to a group of faces, or click to assign a shell property to multiple surfaces that you select using the propagation method.

    If the support you select already has a material assigned to it, the Material field displays the material that is applied to the support.
  4. Optional: If there is no material assignment, or if you want to override the existing material assignment, do the following:
    1. Click .
      The Material Palette appears.
    2. Search for the material you want to assign, and click it.
    3. Click OK to close the Material Palette.
    The Material field displays the newly applied material.
  5. Select a material Behavior that is used in the simulation.
  6. Set Thickness definition to Specified.
  7. For non-axisymmetric models, choose Uniform from the Thickness list, and enter a value for the thickness throughout the entire shell.
  8. Click Table.
    The Thickness Distribution dialog box opens, where you can enter or import the mapped thickness values.
  9. Choose the Data source for the mapped thickness values:
    • Table: Enter or import the mapped data into the table.

    • Referenced document: Select a 3DEXPERIENCE document that contains the mapping data. Click to search for the document in the 3DEXPERIENCE platform database. For details about the required file format, see Mapping Data File Format in the scenario guide for the type of simulation you are creating.

      The app takes into account any changes in the referenced document every time you run the simulation.

  10. Specify the mapped data in the table (if Data source is set to Table):
    • To import the data, right-click anywhere in the table and select Import. For details about the file format required, see Mapping Data File Format in the scenario guide for the type of simulation you are creating.
    • To enter the data manually, double-click in each cell and enter a value, for as many rows as required. For example, enter X-, Y-, and Z-coordinates and the corresponding thickness Value in each row of the table.
  11. Enter the Thickness outside the mapped region. This is a default thickness value.

    The simulation attempts to map all of the source data points and their associated thickness values onto points in the target model. For any target points at which the simulation cannot map a source point, it will substitute this default thickness value.

  12. Select an Axis system definition for the coordinates of the mapped data values.

    • Global: Aligns the local feature triad with the global coordinate system.

    • Local: Aligns the local feature triad with a selected axis system in the model.

      Using a custom Local axis system simplifies the three-dimensional definition of points in space—the X-, Y-, and Z-coordinates are interpreted in the context of the local coordinate system.

  13. Optional: Click Plot Data to display symbols on the model to visualize the locations and magnitudes of the mapped values.

    Tip: If you click any row in the data table, the app highlights the corresponding source point in the model.

  14. Optional: To adjust the search control parameters, expand Search tolerance. See Mapping Search Controls in the scenario guide for the type of simulation you are creating.
  15. Optional: If the materials in your model exhibit directional properties, define their orientation as part of the shell section definition. For more information, see Defining Material Orientations for Shell Sections.

    A material orientation is applied automatically for axisymmetric models.

  16. Specify whether the app integrates the shell section before the analysis or during the analysis. For more information, see Choosing When to Integrate Shell Sections.
  17. Optional: Calculate the average thickness and offset values. For more information, see Averaging Thickness and Offset Values for Shell Sections.
  18. Specify how you want to define the transverse shear stiffness. For more information, see Specifying Transverse Shear Stiffness Directly for Shell Sections.
  19. Select Map thickness to nodes to define the shell thickness at the nodes rather than at the elements.

    Note: Element thickness is calculated as the average of the thickness at each of its nodes.

  20. Click OK.

Define Shell Sections with a Solid or Thin Part Feature Thickness

You can define a shell section that uses the thickness specification from the solid geometry of a midsurface feature or from a thin part feature.

  1. From the Properties section of the action bar, click Shell Section .
  2. Optional: Enter a descriptive Name.
  3. Select a geometry support.

    You apply a shell section to one or more surface geometries. They must be the same surface features that the model uses as the supports for the corresponding mesh part in the FEM representation. You can also use geometry from an ordered geometric set.

    Note: When you mesh an edge fillet whose geoemetry is in a geometry set, apply the shell section property to the mesh feature to assign the section property to the entire region and not just to the fillets.

    For axisymmetric models, you select a cross-section that becomes a surface when the axisymmetric body is rotated. For more information, see About Axisymmetric Simulations.

    You can also assign local shell sections using the tools in the context toolbar. Click to assign a shell property to a group of faces, or click to assign a shell property to multiple surfaces that you select using the propagation method.

    Your choice of geometry support determines the ways in which you can specify the thickness of the shell section:

    • If you choose a midsurface feature as the support, you can choose its associated solid or a different solid to use in determining the shell section thickness.
    • If you choose features other than midsurface features as the support, you must select a solid geometry to extract the thickness and offset for the shell section. This option prevails even if you choose a combination of supports that include both midsurface features and other surface features.

  4. Select a Thickness definition:
    OptionDescription
    From solid Set the shell section thickness based on the thickness attributes of the midsurface feature or from a different solid that you specify. For more information about defining mid surfaces, see the Generative Shape Design Guide.
    Note: If you specify a solid part to define thickness, use a defeatured part for simulation. Otherwise, extra features that remain in the solid can significantly change the thickness calculated for the shell.
    From thin part feature Calculate thickness based on the thin part feature definition. For more information about thin part attributes, see the Simulation Model Preparation Guide.
  5. If you chose a midsurface feature as the geometry support and selected From solid for the thickness definition, specify the thickness using Get thickness from:
    OptionDescription
    Mid-surface The app extracts the thickness of the solid attached to the midsurface feature and uses it as the thickness of the shell section. You cannot edit the extracted thickness definition.
    Solid geometry support Select a different solid geometry support to use its thickness for the shell section, instead of the midsurface feature.
  6. Optional: If the support you select already has a material assigned to it, the Material field displays the material that is applied to the support.
  7. Optional: If there is no material assignment, or if you want to override the existing material assignment, do the following:
    1. Click .
      The Material Palette appears.
    2. Search for the material you want to assign, and click it.
    3. Click OK to close the Material Palette.
    The Material field displays the newly applied material.
  8. Select a material Behavior for the simulation.
  9. Optional: If the materials in your model exhibit directional properties, define their orientation as part of the shell section definition. For more information, see Defining Material Orientations for Shell Sections.

    A material orientation is applied automatically for axisymmetric models.

  10. Specify whether the app integrates the shell section before the analysis or during the analysis. For more information, see Choosing When to Integrate Shell Sections.
  11. Specify how you want to define the transverse shear stiffness. For more information, see Specifying Transverse Shear Stiffness Directly for Shell Sections.
  12. For solid parts, select Map thickness to nodes to define the shell thickness at the nodes rather than at the elements. Mapping thickness to the nodes is not available for thin part features.

    Note: Element thickness is calculated as the average of the thickness at each of its nodes.

  13. Click OK.