Creating composite solid sections

Composite solid sections are used to define the section properties of three-dimensional regions that are composed of layers of different materials in different orientations. For more information, see Defining Composite Solid Elements in Abaqus/Standard.

Context:

Composite solid sections can be used only in Abaqus/Standard. Composite solid sections must be assigned only to three-dimensional brick elements with only displacement degrees of freedom. Composite solid elements are primarily intended for modeling convenience. In most cases you should model a composite section as a shell or continuum shell. However, you should use a composite solid section for the following cases:

  • When the transverse shear effects are predominant.

  • When you cannot ignore the normal stress.

  • When you require accurate interlaminate stresses, such as near localized regions of complex loading or geometry.

If the region to which you assign your composite solid section contains multiple elements through its thickness, each element will contain all the material layers defined in the data table, and the analysis results will not be as expected.

  1. From the main menu bar, select SectionCreate.

    A Create Section dialog box appears.

    Tip: You can also click Create in the Section Manager or select the create section tool in the Property module toolbox.

  2. Enter a section name. For more information on naming objects, see Using basic dialog box components.
  3. Select Solid as the section Category and Composite as the section Type, and click Continue.

    The composite solid section editor appears.

  4. Optionally, enter a layup name. Abaqus/CAE displays this name in a ply stack plot. For more information on naming objects, see Using basic dialog box components.
  5. 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. If you name the material layers, 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.
  6. Each layer of the composite solid section is represented by a row in the data table.

    Note:

    The stacking direction for the composite layers is determined by the material orientation assigned to the solid region. See Assigning a material orientation, for more information.

    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.

    Element Relative Thickness

    The relative thickness of the layer within each element. Abaqus determines the overall section thickness from the element geometry, which may vary from element to element where the section is defined. Hence, the thickness values that you specify for each layer are relative to the thickness of each element. 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. For more information, see Creating a composite layup.

    Orientation Angle

    The orientation. The orientation can be specified either as an angle in degrees or as an orientation name. The orientation angle is measured positive counterclockwise around the normal and relative to the section orientation definition.

    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 solid, you must use the composite layup editor (see Creating and editing composite layups).

    Integration Points

    The number of integration points through the thickness. You can specify only odd numbers.

    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.

    Naming the layers in a composite solid section is optional. However, if you provide a name for any layer, you must provide names for all of the layers in the section.

  7. Click OK to save your changes and to close the composite solid section editor.