Specifying the plies of a continuum shell composite layup

A composite layup is composed of a series of plies. You select the region to which a ply is assigned, and you specify the name, material, relative thickness, orientation, and the number of integration points of each ply. You must specify ply names that are unique throughout the entire model to ensure the correct display of ply-based results. Use the icons above the ply table or click mouse button 3 on the ply table to see a menu that allows you to edit the contents of the table cell and to manipulate the data in the table; for example, you can add and delete plies, pattern plies, and invert plies. You can also read data into the table from a file or write data from the table into a file. For more information, see Using the ply table when defining a composite layup.

  1. From the Composite Layup editor, click the Plies tab.

  2. If the plies in the composite layup are symmetric about a central core, toggle on Make calculated sections symmetric. Enter the plies in the ply table, starting with the bottom ply in the first row and ending with the central ply. During the analysis Abaqus appends plies to the layup definition by repeating the entered plies (including the central ply) in the reverse order to the top of the layup. Each generated ply is labeled in ply stack plots and the output database by adding Sym_ to the beginning of the repeated ply's original name.

    This option cannot be used if the rotation angle for any of the plies in the layup is defined using a discrete field.

  3. For each ply, enter the following data in the ply table:

    Ply Name

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

    Region

    Select the region to which the ply is assigned. You can choose cells from the viewport, or you can select a set that refers to a cell. If you are displaying a meshed dependent part, you can choose solid elements from the viewport or select an element set. To choose elements from the viewport, you must display the native mesh, and you must use the Selection toolbar to enable the selection of 3D Elements from the viewport. You can also select solid elements from a mesh part. For more information, see Displaying a native mesh, and Filtering your selection based on the type of object.

    Material

    The name of the material for this ply. Click mouse button 3, select Edit Material from the menu that appears, and do either of the following:

    • Select the desired material from the list of available materials.

    • Click to create a new material.

    Element Relative Thickness

    The relative ply thickness.

    For continuum shell elements Abaqus determines the thickness from the element geometry, and the thickness may vary through the model for a given layup. Hence, the thickness values that you specify are only relative thicknesses for each ply. The actual thickness of a ply is the element thickness times the fraction of the total thickness that is accounted for by each ply. You do not have to use physical units to specify the thickness ratios for the plies, and the sum of the ply relative thicknesses does not have to add to one.

    Coordinate system

    To define the coordinate system that will be used as the basis for the reference orientation of the ply, do the following:

    1. Click mouse button 3, and select Edit CSYS from the menu that appears.

      Note:

      If you choose Edit Orientation from the menu, you can define both the coordinate system and the rotation angle.

    2. Select the base orientation. You can select the base layup orientation, or you can select a coordinate system. If you select a coordinate system, you must select the axis that defines the normal direction.

    Rotation Angle

    An additional rotation (counterclockwise about the normal direction) for the ply's reference orientation. Enter a uniform rotation directly in the table, or click mouse button 3 and select Edit Rotation Angle to do the following:

    • Select a predefined angle (0, 45, 90, or −45 degrees) to define a uniform rotation.

    • Select Uniform, and enter an Angle to define a uniform rotation.

    • Select a scalar discrete field to define a rotation that varies spatially across the ply. You can also create a new discrete field by clicking .

    Integration Points

    The number of integration points, if you are specifying properties for a composite layup integrated during the analysis.