Specifying the shell parameters of a conventional shell composite layup

From the Composite Layup editor, click the Shell Parameters tab.

Specify the Shell thickness.

• Choose Use section thickness to use the thickness calculated from the individual ply thicknesses.

• Choose Element distribution; and select either an analytical field, labeled with an (A), or an element-based discrete field, labeled with a (D), to define a spatially varying element-based shell thickness. Alternatively, you can click to create a new analytical field or click to create a new discrete field. See The Analytical Field toolset and The Discrete Field toolset for more information.

• Choose Nodal distribution; and select either an analytical field, labeled with an (A), or a node-based discrete field, labeled with a (D), to define a spatially varying node-based shell thickness. Alternatively, you can click to create a new analytical field or click to create a new discrete field. See The Analytical Field toolset and The Discrete Field toolset for more information.

• Choose Determine overall thickness from geometry to have Abaqus/CAE calculate the offset from the thickness defined on the geometry. You must choose From Geometry on the Offset tabbed page.

Specify the Section Poisson's ratio to define the shell thickness behavior. In conventional shell elements that permit finite membrane strains in large-deformation analysis, specifying the section Poisson's ratio causes the shell thickness to change as a function of membrane strains.

• Choose Use analysis default to use the default value. In Abaqus/Standard the default value is 0.5, which will enforce incompressible behavior of the element for membrane strains. In Abaqus/Explicit the default is to base the change in thickness on the element material definition.

• Choose Specify value, and enter a value for the Poisson's ratio. This value must be between −1.0 and 0.5. A value of 0.0 will enforce constant shell thickness, and a negative value will result in an increase in the shell thickness in response to tensile membrane strains.

If you are specifying properties for a composite layup integrated during the analysis, select a method for defining the Temperature variation through the section:

• Choose Linear through thickness to indicate that the temperature at the reference surface and the temperature gradient or gradients through the ply are specified. You can use the Load module to specify these temperatures.

• Choose Piecewise linear over n values to enter the number of temperature points (values) through the ply in the text field provided. You can use the Load module to specify the temperature at each of these points.

Toggle on Density, and enter a value for the density. The mass of the ply includes a contribution from the density in addition to any contribution from the selected material.

For most shell sections Abaqus calculates the transverse shear stiffness values required in the element formulation. If desired, toggle on Specify values from the Transverse Shear Stiffnesses options to include nondefault transverse shear stiffness effects in the section definition, and enter values for $K_{11}$, the shear stiffness of the section in the first direction; $K_{12}$, the coupling term in the shear stiffness of the section; and $K_{22}$, the shear stiffness of the section in the second direction. If either value $K_{11}$ or $K_{22}$ is omitted or given as zero, the nonzero value will be used for both. For more information, see Defining the transverse shear stiffness.