Shell section behavior is defined in terms of the response of the shell section to stretching, bending, shear, and torsion. For more information, see “Shell section behavior,” Section 29.6.4 of the Abaqus Analysis User's Guide. Composite shell sections are composed of layers made of different materials in different orientations.
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.
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 29.6.5 of the Abaqus Analysis User's Guide.
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 elastic material plies; optionally, you can also apply an idealization based on assumptions about the expected behavior or makeup of the shell. Use a pre-integrated 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 29.6.6 of the Abaqus Analysis User's Guide.
The following sections describe how to create a composite shell section:
To create a composite shell section:
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. For more information on naming objects, see “Using basic dialog box components,” Section 3.2.1.
Select Shell as the section Category and Composite as the section Type, and click Continue.
The shell section editor appears.
Choose the Section integration method. Choose During analysis to specify properties for a composite shell section integrated during the analysis. Choose Before analysis to specify properties for a pre-integrated composite shell section.
Enter a layup name. Abaqus/CAE displays this name in a ply stack plot. For more information on naming objects, see “Using basic dialog box components,” Section 3.2.1.
Click 
at the bottom of the shell section editor to define rebar layers in the shell section, as described in “Defining rebar layers,” Section 12.13.19.
Click OK to save your changes and to close the shell section editor.
To specify basic properties for composite shell sections:
On the Basic tabbed page:
Enter the layup name. For more information on naming objects, see “Using basic dialog box components,” Section 3.2.1.
If you are specifying properties for composite shell sections integrated before the analysis, specify the Idealization to apply to the section based on assumptions about the expected behavior or makeup of the shell. For more information, see “Idealizing the section response” in “Using a general shell section to define the section behavior,” Section 29.6.6 of the Abaqus Analysis User's Guide.
Select No idealization to account for the complete stiffness of the shell section as determined by the material assignments and layer composition.
Select Smeared properties if you do not know the exact stacking sequence for the material layers in the composite shell. Contributions from each specified layer are smeared across the entire thickness of the shell, resulting in a general response independent of the stacking sequence.
Select Membrane only if the predominant response of the shell will be in-plane stretching; bending stiffness terms are eliminated from the shell stiffness calculations.
Select Bending only if the predominant response of the shell will be pure bending; membrane stiffness terms are eliminated from the shell stiffness calculations.
If you are specifying properties for composite shell sections integrated during the analysis, 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.
If the layers of material in the section are symmetric about a central core, toggle on Symmetric layers. Enter the material layers in the data table, starting with the bottom layer in the first row and ending with the central layer. During the analysis Abaqus appends layers to the section definition by repeating the entered layers (including the central layer) in the reverse order to the top of the section. Each generated layer is labeled in ply stack plots and the output database by adding Sym_ to the beginning of the repeated layer's original name.
Each layer of the composite shell section is represented by a row in the data table. To add rows to the table, click mouse button three on a row and select Insert Row Before or Insert Row After from the menu that appears. For each layer, enter the following data:
Material
The name of the material forming this layer. Click in the Material column, then click the arrow that appears to display the list of available materials, and select the material forming the layer.
Thickness
The layer thickness. For continuum shell elements Abaqus determines the thickness from the element geometry, and the thickness may vary through the model for a given section definition. Hence, the thickness values that you specify are only relative thicknesses for each layer. The actual thickness of a layer is the element thickness times the fraction of the total thickness that is accounted for by each layer. You do not have to use physical units to specify the thickness ratios for the layers, and the sum of the layer relative thicknesses does not have to add to one. Abaqus uses the shell thickness to estimate certain section properties, such as hourglass stiffness, which are later computed from the element geometry.
Orientation Angle
The orientation, either as a reference to a section orientation definition or as an orientation angle in degrees. The orientation angle, 
, is measured positive counterclockwise around the normal and relative to the section orientation definition.
If either of the two local directions from the section orientation is not in the surface of the shell, is applied after the section orientation has been projected onto the shell surface. If no section orientation has been defined, is measured relative to the default shell local directions.
If you specify an orientation name, Abaqus/CAE assumes a user-defined orientation. You must supply the user subroutine ORIENT that contains the definition of the user-defined orientation for the specified orientation name. You cannot define a variable orientation angle using a discrete field; to define ply-by-ply orientation distributions in a composite shell, you must use the composite layup editor (see “Creating and editing composite layups,” Section 12.14).
Integration Points
The number of integration points through the thickness, if you are specifying properties for composite shell sections integrated during the analysis.
The default number of integration points is 3 for Simpson's rule integration and 2 for Gauss quadrature integration.
If you are using the Simpson integration rule, you can specify only odd numbers.
If you are using the Gauss integration rule, you can specify numbers less than or equal to 7.
Ply Name
The name of the layer. Abaqus/CAE displays this name when you are viewing the composite plies in the Visualization module and in a ply stack plot.
To specify advanced properties for composite shell sections:
On the Advanced tabbed page:
Specify the Shell thickness.
Choose Use section thickness to use the thickness calculated from the individual layer 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 Chapter 58, “The Analytical Field toolset,” and Chapter 63, “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 Chapter 58, “The Analytical Field toolset,” and Chapter 63, “The Discrete Field toolset,” for more information.
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 composite 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 
, 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.