Shell section behavior is defined in terms of the response of the beam section to stretching, bending, shear, and torsion. For more information, see “Shell section behavior,” Section 23.6.4 of the ABAQUS Analysis User's Manual.
When you create shell sections, you must choose a section integration method. You can choose to provide the section property data before the analysis (a pre-integrated shell section) or to have ABAQUS calculate (integrate) the cross-sectional behavior from section integration points during the analysis. The following sections describe how to define a homogeneous shell section for each integration method:
Linear moment-bending and force-membrane strain relationships can be defined using pre-integrated shell sections. In this case all calculations are done in terms of section forces and moments. The section properties are specified by an elastic material. Use this type of shell section if the response of the shell is linear elastic and its behavior is not dependent on changes in temperature or predefined field variables. For more information, see “Using a general shell section to define the section behavior,” Section 23.6.6 of the ABAQUS Analysis User's Manual.
To specify properties for pre-integrated homogeneous shell sections:
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 Homogeneous as the section Type, and click Continue.
The shell section editor appears.
Select Before analysis as the Section integration method.
On the Basic tabbed page:
Enter a value for the Shell thickness. In continuum shells this value is used to estimate certain section properties, such as hourglass stiffness, which are later computed from the element geometry.
Select a material for the shell section. If desired, click Create to create a material; see “Creating or editing a material,” Section 12.6.1, for more information.
On the Advanced 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:
Toggle on Use analysis default to use the default value of 0.5, which will enforce incompressible behavior of the element for membrane strains.
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.
For most shell sections ABAQUS will calculate the transverse shear stiffness values required in the element formulation. If desired, toggle on Specify transverse shear to include nondefault transverse shear stiffness effects in the section definition, and enter values for 
, the shear stiffness of the section in the first direction; 
, the coupling term in the shear stiffness of the section; and 
, the shear stiffness of the section in the second direction. If either value or is omitted or given as zero, the nonzero value will be used for both.
Click OK to save your changes and to close the shell section editor.
Shell sections integrated during analysis allow the cross-sectional behavior to be calculated by numerical integration through the shell thickness, thus providing complete generality in material modeling. Any number of material points can be defined through the thickness, and the material response can vary from point to point. This type of shell section is generally used with nonlinear material behavior in the section. It must be used with shells that provide for heat transfer. For more information, see “Using a shell section integrated during the analysis to define the section behavior,” Section 23.6.5 of the ABAQUS Analysis User's Manual.
To specify properties for homogeneous shell sections integrated during analysis:
From the main menu bar, select SectionCreate.
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 Homogeneous as the section Type, and click Continue.
The shell section editor appears.
Choose During analysis as the Section integration method.
On the Basic tabbed page:
Enter a value for the Shell thickness. In continuum shells this value is used to estimate certain section properties, such as hourglass stiffness, which are later computed using the actual thickness computed from the element geometry.
Select a material for the shell section. If desired, click Create to create a material; see “Creating or editing a material,” Section 12.6.1, for more information. Linear or nonlinear material behavior can be associated with the section definition. However, if the material response is linear, a more economical approach is to use a generalized shell section.
Select the Thickness integration rule.
Choose Simpson to use Simpson's rule for the shell section integration.
Choose Gauss to use Gauss quadrature for the shell section integration.
The default number of integration points through the thickness is 5 for Simpson's rule integration and 3 for Gauss quadrature integration. To specify a new value for the number of integration points, you can type the number directly or click the upward or downward arrow in the Thickness integration points text field.
If you are using the Simpson integration rule, you can specify only odd numbers ranging from 3 to 15.
If you are using the Gauss integration rule, you can specify numbers ranging from 2 to 7.
On the Advanced 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:
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.
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.
For most shell sections ABAQUS will calculate the transverse shear stiffness values required in the element formulation. If desired, toggle on Specify transverse shear to include nondefault transverse shear stiffness effects in the section definition, and enter values for , the shear stiffness of the section in the first direction; , the coupling term in the shear stiffness of the section; and , the shear stiffness of the section in the second direction. If either value or is omitted or given as zero, the nonzero value will be used for both.
Click Rebar Layers at the bottom of the shell section editor to define rebar layers in the shell section, as described in “Defining rebar layers,” Section 12.11.13.
Click OK to save your changes and to close the shell section editor.