Creating solid composite layups

In Abaqus/Standard solid elements can include several layers of different materials for the analysis of laminated composite solids; however, in Abaqus/Explicit solid elements can be composed only of a single homogeneous material. The use of composite solids is limited to three-dimensional brick elements that have only displacement degrees of freedom. Composite solid elements are primarily intended for modeling convenience. They usually do not provide a more accurate solution than composite shell elements. For more information, see Defining composite solid elements in Abaqus/Standard, and Modeling thick composites with solid elements in Abaqus/Standard.

  1. From the main menu bar, select CompositeCreate.

    A Create Composite Layup dialog box appears.

    Tip: You can also click Create in the Composite Layup Manager or select the create composite layup tool in the Property module toolbox.

  2. Enter a composite layup name. For more information on naming objects, see Using basic dialog box components.

  3. Specify the initial ply count. When the composite layup editor appears, it will contain a row for each ply; however, you can use the editor to subsequently add or delete plies.

  4. Select Solid as the Element Type, and click Continue.

    The composite layup editor appears.

  5. Enter a description of the layup. Abaqus/CAE displays this description in the composite layup manager.

  6. Do one of the following to specify the layup orientation:

    • Select Coordinate system to select an existing coordinate system (or create a new coordinate system and select it), and do the following:

      1. Choose the axis that represents the Rotation axis.

      2. Specify an additional rotation. The selected coordinate system is rotated through this angle about the selected axis. You can specify an angle, or you can select an existing scalar discrete field that defines an angle that is varying spatially across the layup. Abaqus/CAE allows you to select only valid discrete fields, which, for an additional rotation, are scalar discrete fields applied to elements. You can also create a new discrete field by clicking . For more information, see The Discrete Field toolset.”

    • Select Discrete to define a discrete orientation, and do the following:

      1. Click .

      2. In the Edit Discrete Orientation dialog box that appears, define the normal axis and primary axis using the procedure described in Using discrete orientations for material orientations and composite layup orientations.

      3. Choose the axis that represents the Rotation axis.

      4. Specify an additional rotation. The orientation is rotated through this angle about the selected normal axis. You can specify an angle, or you can select or create a scalar discrete field that defines an angle that is varying spatially across the layup. Abaqus/CAE allows you to select only valid discrete fields, which, for an additional rotation, are scalar discrete fields applied to elements. You can also create a new discrete field by clicking . For more information, see The Discrete Field toolset.”

    • Select User-defined to define the orientation in user subroutine ORIENT. This option is valid only for Abaqus/Standard analyses. See the following sections for more information:

    • Select the name of an orientation discrete field to specify a coordinate system that is varying spatially across the layup. You can also create a new discrete field by clicking to the right of the Definition field. For more information, see The Discrete Field toolset.” After selecting the discrete field, you must do the following:

      1. Choose the axis that represents the Rotation axis.

      2. Specify an additional rotation. The selected coordinate system is rotated through this angle about the selected axis. You can specify an angle, or you can select or create a scalar discrete field that defines an angle that is varying spatially across the layup.

    The layup orientation is the reference orientation for any ply that uses the default orientation system (indicated by <Layup> in the CSYS column of the ply table). This orientation will be used for material calculations and stress output in the individual plies, for the section forces output, and for the transverse shear stiffness. You can specify a different orientation for the individual plies of a solid composite layup by specifying a reference orientation and/or a rotation angle. For more information, see Understanding composite layups and orientations.

  7. Choose one of the following to specify the stacking direction of the solid elements with respect to a pair of element faces:

    • Element direction 1

    • Element direction 2

    • Element direction 3

    You can use the Query toolset to determine the mesh stack orientation. However, the displayed orientations account for only the sweep path; they do not account for changes to the stacking direction as described above. For more information on the Query toolset, see Using the Query toolset to query the model. For more information on mesh stack directions, see Defining the stacking and thickness direction.