Abaqus models a continuum shell composite layup using continuum shell elements that fully discretize each ply but have a kinematic behavior that is based on shell theory. Continuum shell composite layups are composed of plies made of different materials in different orientations. A layup can contain a different number of plies in different regions. For more information, see Chapter 23, “Composite layups.”
Continuum shell composite layups are expected to have a single element through their thickness, and that single element contains multiple plies that are defined in the ply table. If the region to which you assign your continuum shell composite layup contains multiple elements, each element will contain the plies defined in the ply table, and the analysis results will not be as expected.
You choose the stacking direction of the continuum shell elements in the layup, which allows Abaqus to model the through-thickness response more accurately. In addition, continuum shell composite layups take into account double-sided contact and thickness changes, which provides more accurate contact modeling than conventional shell composite layups. For more information, see “Shell section behavior,” Section 29.6.4 of the Abaqus Analysis User's Guide.
When you create continuum shell composite layups, you must choose a section integration method. You can choose to provide the section property data before the analysis (a pre-integrated continuum shell composite layup) or to have Abaqus calculate (integrate) the cross-sectional behavior from integration points during the analysis.
Continuum shell composite layups integrated during the analysis allow the cross-sectional behavior to be calculated by numerical integration through the continuum 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. You generally use continuum shell elements integrated during analysis when the composite layup includes nonlinear material behavior. You must use continuum shell elements integrated during analysis to model 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 continuum shell composite layups. In this case all calculations are done in terms of section forces and moments. The section properties are specified by an elastic material; optionally, you can also apply an idealization based on assumptions about the expected behavior or makeup of the layup. You should use pre-integrated continuum shell composite layups if the response of the layup 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.
After you have created a continuum shell composite layup, you can use a ply stack plot to view a graphical representation of a core sample through a region of the layup. For more information, see Chapter 53, “Viewing a ply stack plot.”
The following sections describe how to create a continuum shell composite layup:
You can define a continuum shell composite layup with a specified stacking direction that is composed of plies made of one or more materials. For each ply of the layup, you specify the name, material, relative thickness, orientation, and the number of integration points. In addition, you select the region to which the ply is assigned. For more information, see “Defining a composite shell section” in “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5 of the Abaqus Analysis User's Guide.
To create a continuum shell composite layup:
From the main menu bar, select Composite
Create.
A Create Composite Layup dialog box appears.
Tip:
You can also click Create in the Composite Layup Manager or select the create composite layup tool 
in the Property module toolbox.
Enter a composite 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.
Specify the initial ply count. When the composite layup editor appears, it will contain a row for each ply; however, you can use the editor to subsequently add or delete plies.
Select Continuum Shell as the Element Type, and click Continue.
The composite layup editor appears.
Enter a description of the layup. Abaqus/CAE displays this description in the composite layup manager.
Do one of the following to specify the layup orientation:
Select Part global to use the part's coordinate system, and choose the axis that represents the Normal direction.
Select Coordinate system to select an existing coordinate system (or create a new coordinate system and select it), and do the following:
Choose the axis that represents the Normal direction.
Specify an additional rotation. The selected coordinate system is rotated through this angle about the selected axis. You can specify an angle, or you can select an existing scalar discrete field that defines an angle that is varying spatially across the layup. Abaqus/CAE allows you to select only valid discrete fields, which, for an additional rotation, are scalar discrete fields applied to elements. You can also create a new discrete field by clicking 
. For more information, see Chapter 63, “The Discrete Field toolset.”
Select Discrete to define a discrete orientation, and do the following:
Click 
.
In the Edit Discrete Orientation dialog box that appears, define the normal axis and primary axis using the procedure described in “Using discrete orientations for material orientations and composite layup orientations,” Section 12.16.
Choose the axis that represents the Normal direction.
Specify an additional rotation. The orientation is rotated through this angle about the selected normal axis. You can specify an angle, or you can select or create a scalar discrete field that defines an angle that is varying spatially across the layup. Abaqus/CAE allows you to select only valid discrete fields, which, for an additional rotation, are scalar discrete fields applied to elements. You can also create a new discrete field by clicking . For more information, see Chapter 63, “The Discrete Field toolset.”
Select User-defined to define the orientation in user subroutine ORIENT. This option is valid only for Abaqus/Standard analyses. See the following sections for more information:
Select the name of an orientation discrete field to specify a coordinate system that is varying spatially across the layup. You can also create a new discrete field by clicking to the right of the Definition field. For more information, see Chapter 63, “The Discrete Field toolset.” After selecting the discrete field, you must do the following:
Choose the axis that represents the Normal direction.
Specify an additional rotation. The selected coordinate system is rotated through this angle about the selected axis. You can specify an angle, or you can select or create a scalar discrete field that defines an angle that is varying spatially across the layup.
Choose one of the following to specify the stacking direction of the continuum shell elements:
Element direction 1
Element direction 2
Element direction 3
Layup orientation. The stacking direction is the normal to the layup orientation.
Choose one of the following Section integration methods:
Choose During analysis to specify properties for a continuum shell composite layup integrated during the analysis.
Choose Before analysis to specify properties for a pre-integrated continuum shell composite layup.
If you are specifying properties for a composite layup integrated before the analysis, specify the Idealization to apply to the shell based on assumptions about the expected behavior or makeup of the layup. 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 as determined by the material assignments and ply composition.
Select Smeared properties if you do not know the exact stacking sequence for the plies in the composite layup. Contributions from each specified ply are smeared across the entire thickness of the layup, 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 a composite layup 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.
When you have finished defining the continuum shell composite layup, click OK to save your changes and to close the editor.
A composite layup is composed of a series of plies. You select the region to which a ply is assigned, and you specify the name, material, relative thickness, orientation, and the number of integration points of each ply. You must specify ply names that are unique throughout the entire model to ensure the correct display of ply-based results. Use the icons above the ply table or click mouse button 3 on the ply table to see a menu that allows you to edit the contents of the table cell and to manipulate the data in the table; for example, you can add and delete plies, pattern plies, and invert plies. You can also read data into the table from a file or write data from the table into a file. For more information, see “Using the ply table when defining a composite layup,” Section 12.14.1.
To specify the plies of a continuum shell composite layup:
From the Composite Layup editor, click the Plies tab.
If the plies in the composite layup are symmetric about a central core, toggle on Make calculated sections symmetric. Enter the plies in the ply table, starting with the bottom ply in the first row and ending with the central ply. During the analysis Abaqus appends plies to the layup definition by repeating the entered plies (including the central ply) in the reverse order to the top of the layup. Each generated ply is labeled in ply stack plots and the output database by adding Sym_ to the beginning of the repeated ply's original name.
This option cannot be used if the rotation angle for any of the plies in the layup is defined using a discrete field.
For each ply, enter the following data in the ply table:
Ply Name
The name of the ply. Abaqus/CAE displays this name when you are viewing the composite layup in the Visualization module and in a ply stack plot.
Region
Select the region to which the ply is assigned. You can choose cells from the viewport, or you can select a set that refers to a cell. If you are displaying a meshed dependent part, you can choose solid elements from the viewport or select an element set. To choose elements from the viewport, you must display the native mesh, and you must use the Selection toolbar to enable the selection of 3D Elements from the viewport. You can also select solid elements from a mesh part. For more information, see “Displaying a native mesh,” Section 17.3.11, and “Filtering your selection based on the type of object,” Section 6.3.2.
Material
The name of the material for this ply. Click mouse button 3, select Edit Material from the menu that appears, and do either of the following:
Select the desired material from the list of available materials.
Click 
to create a new material.
Element Relative Thickness
The relative ply thickness.
For continuum shell elements Abaqus determines the thickness from the element geometry, and the thickness may vary through the model for a given layup. Hence, the thickness values that you specify are only relative thicknesses for each ply. The actual thickness of a ply is the element thickness times the fraction of the total thickness that is accounted for by each ply. You do not have to use physical units to specify the thickness ratios for the plies, and the sum of the ply relative thicknesses does not have to add to one.
Coordinate system
To define the coordinate system that will be used as the basis for the reference orientation of the ply, do the following:
Click mouse button 3, and select Edit CSYS from the menu that appears.
Note: If you choose Edit Orientation from the menu, you can define both the coordinate system and the rotation angle.
Select the base orientation. You can select the base layup orientation, or you can select a coordinate system. If you select a coordinate system, you must select the axis that defines the normal direction.
Rotation Angle
An additional rotation (counterclockwise about the normal direction) for the ply's reference orientation. Enter a uniform rotation directly in the table, or click mouse button 3 and select Edit Rotation Angle to do the following:
Select a predefined angle (0, 45, 90, or –45 degrees) to define a uniform rotation.
Select Uniform, and enter an Angle to define a uniform rotation.
Select a scalar discrete field to define a rotation that varies spatially across the ply. You can also create a new discrete field by clicking .
Integration Points
The number of integration points, if you are specifying properties for a composite layup integrated during the analysis.
To specify the shell parameters of a continuum shell composite layup:
From the Composite Layup editor, click the Shell Parameters tab.
Specify the Section Poisson's ratio to define the shell thickness behavior:
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.
Toggle on Thickness modulus, and enter a value for the thickness modulus. If you do not enter a value, Abaqus assumes the effective thickness modulus is twice the initial in-plane shear modulus based on the material definition.
If you are specifying properties for a composite layup 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 ply 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 ply 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 density. The mass of the ply includes a contribution from the density in addition to any contribution from the selected material.
For most continuum shell composite layups Abaqus calculates 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 composite layup definition, and enter values for 
, the shear stiffness in the first direction; 
, the coupling term in the shear stiffness; and 
, the shear stiffness in the second direction. If either value or is omitted or given as zero, the nonzero value will be used for both. For more information, see “Defining the transverse shear stiffness” in “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5 of the Abaqus Analysis User's Guide.
To specify the display of selected plies:
From the Composite Layup editor, click the Display tab.
Choose how Abaqus/CAE highlights the plies that you selected in the ply table:
Choose On to highlight the selected plies.
Choose Off to stop highlighting the selected plies. If you have a large number of plies in your model, you may want to turn off highlighting to increase performance.
Choose which orientation Abaqus/CAE displays on the selected plies:
Choose Ply to display the ply orientation on the selected plies.
Choose Layup to display the layup orientation on the selected plies.
Choose None to stop displaying an orientation.
Specify which orientation vectors you want to display on the selected plies. You can toggle the display of vectors in the 1-direction, the 2-direction, and the 3- (or normal) direction, as well as the reference direction that shows the 1-direction before rotation of the ply's material directions.