Creating a 2D Property Enhancement

A 2D property defines the material associated with a surface and its thickness. You can create a 2D property using the 2D Property tool, which is described in more detail in the Creating 2D Properties. A 2D property enhancement assigns additional property behavior to a shell or membrane. 2D property enhancements are also used to assign continuum shell behavior to solids. For more information, see Assigning Continuum Shell Properties to Solids.

The section integration for a 2D property enhancement can use either of the following approaches:

Creating a 2D Property Enhancement: Assigns additional 2D property behavior to an existing 2D or 3D property.

This task shows you how to add a 2D property enhancement to a Nonlinear Structural case or to an Explicit Dynamics case.

  1. Select Start>Analysis & Simulation>Nonlinear Structural Analysis from the menu bar to enter the Nonlinear Structural Analysis workbench.

  2. If necessary, set a Nonlinear Structural case or an Explicit Dynamics case to be the current case. If the case is not empty, it must contain structural analysis procedures.

  3. Click the 2D Property Enhancement icon .

    The 2D Property Enhancement dialog box appears, and a 2D Property Enhancement object appears in the specification tree under the current Nonlinear and Thermal Properties.

  4. You can change the 2D property enhancement identifier by editing the Name field. This name will be used in the specification tree.

  5. In the specification tree, select a 2D Property or a 3D Property to which the enhancement will be applied.

    The Property field is updated to reflect your selection.

  6. Specify the Type:

    • Membrane: The shell is made of a single linear elastic material and has no bending stiffness. The strength of a membrane is all in the plane of the surface.

    • Homogeneous (the default): The shell is made of a single linear elastic material.

    • Composite: The shell is composed of layers with different linear elastic material behaviors.

The remaining options depend on your choice of type. If you selected Membrane, the following task shows you how to complete the 2D property enhancement. If you selected Homogeneous or Composite, see the task immediately following this one.

  1. Enter the section Poisson's ratio. The default value is 0.5, which enforces incompressible behavior.

  2. Click OK in the 2D Property Enhancement dialog box.

This task shows you how to complete the 2D property enhancement definition for the Homogeneous and Composite types. If you selected the Membrane type, see the previous task.

  1. If you selected the Composite shell type, select a layup from the specification tree. The layup defines the material name, thickness, and orientation of each layer of the composite. See Creating a Layup for more information.

  2. Shell elements use material orientations that are local to each element. Element output variables, such as stress and strain, are defined in terms of these local material orientations. You can use the default material orientation, or you can define the material orientation by specifying the following:

    • The coordinate system type—rectangular, cylindrical, or spherical.

    • A selected coordinate system. If the desired coordinate system does not exist, go to the Part Design workbench, and select Insert>Axis from the menu bar to create the coordinate system.

    • The axis of the coordinate system representing the approximate shell normal.

    • An additional rotation of the local coordinate system about the shell normal.

    Default material orientations are described in Conventions in the Abaqus Introduction & Spatial Modeling Guide. User-defined material orientations are described in Orientations in the Abaqus Introduction & Spatial Modeling Guide.

  3. Specify an Offset as a fraction of shell thickness. The offset determines the distance from the shell's midsurface to the reference surface containing the elements' nodes (see Defining the initial geometry of conventional shell elements in the Abaqus Elements Guide for more information). Positive values of the offset are in the positive normal direction: when the offset is set equal to 0.5, the top surface of the shell is the reference surface; when the offset is set equal to –0.5, the bottom surface of the shell is the reference surface. The default offset is 0, which indicates that the shell's midsurface is the reference surface.

  4. Specify when Abaqus should perform the numerical integration through the thickness of the shell section by choosing During analysis (the default) or Before analysis. If you choose to perform the integration during the analysis, do the following:

    1. Specify the section integration rule by choosing Simpson (the default) to use Simpson's rule or Gauss to use Gauss quadrature. You cannot use Gauss quadrature with heat transfer.

    2. Enter the number of integration points to be used through the shell section. The default integration method is Simpson’s rule with five integration points through the thickness of each layer. The default value for Gauss quadrature is three integration points. (See Using a shell section integrated during the analysis to define the section behavior in the Abaqus Elements Guide for more information.)

      Note:  If you are using the shell property enhancement to define a layup of composite materials, you must select Simpson's rule and three integration points. CATIA V5 supports only three integration points through the thickness of a lamina.

  5. Specify how the temperature varies across the shell section by choosing Linear through thickness (the default) or Piecewise linear. If you choose Piecewise linear, enter the number of equally spaced points across the section.

  6. Enter the section Poisson's ratio. The default value is 0.5, which enforces incompressible behavior.

  7. Click OK in the 2D Property Enhancement dialog box.