Conventional 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.” Abaqus models a shell composite layup using conventional shell elements that discretize only the reference surface of each ply. Shell section behavior is defined in terms of the response of the shell section to stretching, bending, twist, and transverse shear. For more information, see “Shell section behavior,” Section 29.6.4 of the Abaqus Analysis User's Guide.
When you create conventional 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 shell section) or to have Abaqus calculate (integrate) the cross-sectional behavior from section integration points during the analysis.
Conventional shell composite layups 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. You generally use shell elements integrated during analysis when the composite layup includes nonlinear material behavior. You must use 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 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 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 conventional 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 shell composite layup:
You can define a conventional shell composite layup composed of plies made of one or more materials. For each ply of the layup, you specify the name, material, thickness, orientation, and the number of integration points. In addition, you select the region to which the ply is assigned. For more information, see “Shell section behavior,” Section 29.6.4 of the Abaqus Analysis User's Guide.
To create a conventional 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. The first row of the ply table corresponds to the bottom ply of the layup.
Select Conventional 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.
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 Section integration methods:
Choose During analysis to specify properties for a shell composite layup integrated during the analysis.
Choose Before analysis to specify properties for a pre-integrated 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 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, 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 conventional 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 thickness or 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 faces from the viewport, or you can select a set that refers to a face. If you are displaying a meshed dependent part, you can choose shell 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 2D Elements. You can also select shell 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.
Thickness
The ply thickness. Enter a uniform thickness directly in the table, or click mouse button 3 and select Edit Thickness to do the following:
Choose Specify Value to enter a uniform thickness for the ply.
Choose Distribution and select a scalar discrete field to specify a thickness that varies spatially across the ply.
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.
In most cases you can use the midsurface of an element to indicate the reference surface. However, in some cases you need to define the reference surface as offset from the midsurface of the elements. For example, a model imported from a CAD system might assume that the shell is located at the top or bottom surface of the elements. In addition, you can specify a shell offset that defines a more precise surface geometry for contact problems where shell thickness is important. The offset value is defined as a fraction of the total thickness measured from the midsurface to the reference surface.
Positive values of the offset are in the positive element normal direction. When the offset is set equal to 0.5, the top surface of the element is the reference surface. When the offset is set equal to –0.5, the bottom surface is the reference surface. The default offset is 0, which indicates that the middle surface of the element is the reference surface. Figure 12–18 shows an offset to the top surface of the element.
For more information, see “Defining the initial geometry of conventional shell elements,” Section 29.6.3 of the Abaqus Analysis User's Guide. You can use a discrete field to model elements with continuously varying offsets. For more information, see Chapter 63, “The Discrete Field toolset.”
To specify the offset of a conventional shell composite layup:
From the Composite Layup editor, click the Offset tab.
Do one of the following:
Choose the Middle surface, Top surface, or Bottom surface to represent the reference surface.
Choose Specify offset ratio, and enter a number.
Choose Distribution, and select an existing scalar discrete field that defines an offset that is varying spatially across the layup. Abaqus/CAE allows you to select only valid discrete fields, which, for an offset, 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.”
To specify the shell parameters of a conventional shell composite layup:
From the Composite Layup editor, click the Shell Parameters tab.
Specify the Shell thickness.
Choose Use section thickness to use the thickness calculated from the individual ply 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.
Choose 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.
Choose 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.
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 shell sections 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 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. 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.
