From the main menu bar, select .
A Create Section dialog box appears.
Enter a section name. For more information on naming objects, see Using basic dialog box components. Select Shell as the section Category and Membrane as the section Type, and click Continue. The membrane section editor appears. Select a material for the membrane section. If desired, click Create to create a material; see Creating or editing a material, for more information. Specify the Membrane thickness.
-
Choose Value, and enter a value for the membrane thickness.
-
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 membrane 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.
Specify the Section Poisson's ratio to define how the membrane thickness will change with deformation.
-
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. 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 thickness, and a negative value will result in an increase in the thickness in response to tensile membrane strains.
Click  at the bottom of the membrane section editor to define rebar layers in the membrane section, as described in Defining rebar layers. Click OK to save your changes and to close the membrane section editor.
|
in the Property module toolbox.