Shell elements and membrane elements are used to model structures in which one dimension, the thickness, is significantly smaller than the other dimensions. Membrane elements are discussed in Assigning Membrane Properties to Surfaces. Two types of shell elements are available in Abaqus for CATIA V5: conventional shell elements and continuum shell elements. Conventional shell elements model a relatively thin surface by defining two-dimensional elements along with the shell normal direction. The nodes of a conventional shell element do not define the shell thickness; you specify the thickness of the shell when you assign a 2D Property to the shell. Continuum shell elements, on the other hand, resemble three-dimensional solid elements in that they model an entire three-dimensional body, and their thickness is determined from the element nodal geometry. However, continuum shell elements are formulated so that their kinematic and constitutive behavior is similar to conventional shell elements. Figure 8–8 illustrates the difference between conventional and continuum shell elements.

Conventional shell elements have displacement and rotational degrees of freedom; continuum shell elements have only displacement degrees of freedom. Continuum shell elements are more accurate in contact modeling than conventional shell elements, since they employ two-sided contact calculated at the surface of the element. Continuum shell elements also take into account changes in element thickness during contact. For thin-shell applications, conventional shell elements provide superior performance. See Shell elements: overview in the Abaqus Elements Guide, and Choosing a shell element in the Abaqus Elements Guide for more information.

Because continuum shell elements have a thickness direction associated with them, you must orient the elements correctly. You define the element stacking direction and thickness direction by assigning a material orientation to a 2D Property Enhancement and by specifying the approximate shell normal. The thickness direction strain is computed from the element nodal displacements, which in turn depend on the effective thickness modulus and the section Poisson's ratio. See Defining the thickness modulus in continuum shell elements in Using a general shell section to define the section behavior in the Abaqus Elements Guide for more information.

You assign continuum shell elements to a solid that has been meshed with either hexahedral or wedge elements. It is recommended that you create the continuum shell elements by meshing a face and by extruding the two-dimensional elements through the thickness of the solid. In effect, you are thickening a meshed shell. For example, you can use the Sweep 3D tool in the Advanced Meshing Tools workbench. Unlike conventional shells, continuum shell elements can be stacked through the thickness of the shell to provide more refined through-thickness response. A layer of a single element is adequate for capturing bending; however, stacking continuum shell elements allows for a richer transverse shear stress and force prediction.