Specifying advanced properties for homogeneous shell section

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:

  • Toggle on 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.

  • Toggle on 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.

• In continuum shell elements specifying the section Poisson's ratio defines the thickness behavior for both small- and large-displacement analysis:

  • Toggle on Use analysis default to indicate that the change in thickness is based on the element material definition.

  • Toggle on Specify value, and enter a value for the Poisson's ratio to cause the shell thickness to change as a function of membrane strains. This value must be between −1.0 and 0.5. A value of 0.5 cannot be used with continuum shells. 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.

For continuum shell elements, toggle on Thickness modulus, and enter a value for the effective thickness modulus. If you do not specify a thickness modulus, Abaqus will try to compute it based on the initial elastic material properties.

If you are specifying properties for homogeneous shell sections 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 section 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 section 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 mass per unit surface area of the shell. The mass of the shell includes a contribution from the density in addition to any contribution from the selected material.

For most shell sections Abaqus will calculate 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.

If you are specifying properties for homogeneous shell sections integrated during the analysis, click at the bottom of the shell section editor to define rebar layers in the shell section, as described in Defining rebar layers.

Click OK to save your changes and to close the shell section editor.