Specifying basic properties for composite shell sections

You can specify basic properties for composite shell sections.

Context:

On the Basic tabbed page:

  1. Enter the layup name. For more information on naming objects, see Using basic dialog box components.

  2. If you are specifying properties for composite shell sections integrated before the analysis, specify the Idealization to apply to the section based on assumptions about the expected behavior or makeup of the shell. For more information, see Idealizing the section response.

    • Select No idealization to account for the complete stiffness of the shell section as determined by the material assignments and layer composition.

    • Select Smeared properties if you do not know the exact stacking sequence for the material layers in the composite shell. Contributions from each specified layer are smeared across the entire thickness of the shell, resulting in a general response independent of the stacking sequence.

    • Select Membrane only if the predominant response of the shell will be in-plane stretching; bending stiffness terms are eliminated from the shell stiffness calculations.

    • Select Bending only if the predominant response of the shell will be pure bending; membrane stiffness terms are eliminated from the shell stiffness calculations.

  3. If you are specifying properties for composite shell sections integrated during the analysis, select the Thickness integration rule.

    • Choose Simpson to use Simpson's rule for the shell section integration.

    • Choose Gauss to use Gauss quadrature for the shell section integration.

    See Defining the shell section integration, for more information.

  4. If the layers of material in the section are symmetric about a central core, toggle on Symmetric layers. Enter the material layers in the data table, starting with the bottom layer in the first row and ending with the central layer. During the analysis Abaqus appends layers to the section definition by repeating the entered layers (including the central layer) in the reverse order to the top of the section. Each generated layer is labeled in ply stack plots and the output database by adding Sym_ to the beginning of the repeated layer's original name.

  5. Each layer of the composite shell section is represented by a row in the data table. To add rows to the table, click mouse button three on a row and select Insert Row Before or Insert Row After from the menu that appears. For each layer, enter the following data:

    Material

    The name of the material forming this layer. Click in the Material column, then click the arrow that appears to display the list of available materials, and select the material forming the layer.

    Thickness

    The layer thickness. For continuum shell elements Abaqus determines the thickness from the element geometry, and the thickness may vary through the model for a given section definition. Hence, the thickness values that you specify are only relative thicknesses for each layer. The actual thickness of a layer is the element thickness times the fraction of the total thickness that is accounted for by each layer. You do not have to use physical units to specify the thickness ratios for the layers, and the sum of the layer relative thicknesses does not have to add to one. Abaqus uses the shell thickness to estimate certain section properties, such as hourglass stiffness, which are later computed from the element geometry.

    Orientation Angle

    The orientation, either as a reference to a section orientation definition or as an orientation angle in degrees. The orientation angle, ϕ, is measured positive counterclockwise around the normal and relative to the section orientation definition.

    If either of the two local directions from the section orientation is not in the surface of the shell, ϕ is applied after the section orientation has been projected onto the shell surface. If no section orientation has been defined, ϕ is measured relative to the default shell local directions.

    If you specify an orientation name, Abaqus/CAE assumes a user-defined orientation. You must supply the user subroutine ORIENT that contains the definition of the user-defined orientation for the specified orientation name. You cannot define a variable orientation angle using a discrete field; to define ply-by-ply orientation distributions in a composite shell, you must use the composite layup editor (see Creating and editing composite layups).

    Integration Points

    The number of integration points through the thickness, if you are specifying properties for composite shell sections integrated during the analysis.

    The default number of integration points is 3 for Simpson's rule integration and 2 for Gauss quadrature integration.

    • If you are using the Simpson integration rule, you can specify only odd numbers.

    • If you are using the Gauss integration rule, you can specify numbers less than or equal to 7.

    Ply Name

    The name of the layer. Abaqus/CAE displays this name when you are viewing the composite plies in the Visualization module and in a ply stack plot.