Membrane sections are used to define the section properties of thin surfaces in space that offer strength in the plane of the surface but have no bending stiffness. For more information, see “Membrane elements,” Section 23.1.1 of the ABAQUS Analysis User's Manual.
To specify membrane section properties:
From the main menu bar, select Section
Create.
A Create Section dialog box appears.
Tip:
You can also click Create in the Section Manager or select the create section tool 
in the Property module toolbox.
Enter a section name of your choice. For more information on naming objects, see “Using basic dialog box components,” Section 3.2.1.
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,” Section 12.6.1, for more information.
Enter a value for the Membrane thickness.
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 Rebar Layers at the bottom of the membrane section editor to define rebar layers in the membrane section, as described in “Defining rebar layers,” Section 12.11.13.
Click OK to save your changes and to close the membrane section editor.