In most cases, you should model a composite solid as a shell or continuum shell composite layup. However, you should use a solid composite layup for the following cases:
When the transverse shear effects are predominant.
When you cannot ignore the normal stress.
When you require accurate interlaminar stresses, such as near localized regions of complex loading or geometry.
Solid 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 solid 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.
The following sections describe how to create a solid composite layup:
In Abaqus/Standard solid elements can include several layers of different materials for the analysis of laminated composite solids; however, in Abaqus/Explicit solid elements can be composed only of a single homogeneous material. The use of composite solids is limited to three-dimensional brick elements that have only displacement degrees of freedom. Composite solid elements are primarily intended for modeling convenience. They usually do not provide a more accurate solution than composite shell elements. For more information, see “Defining composite solid elements in Abaqus/Standard” in “Solid (continuum) elements,” Section 28.1.1 of the Abaqus Analysis User's Guide, and “Modeling thick composites with solid elements in Abaqus/Standard” in “Solid (continuum) elements,” Section 28.1.1 of the Abaqus Analysis User's Guide.
To create a solid 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. 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 Solid 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 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 Rotation axis.
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 Rotation axis.
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 Rotation axis.
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 solid elements with respect to a pair of element faces:
Element direction 1
Element direction 2
Element direction 3
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 solid 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.
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 solid elements Abaqus determines the thickness from the part 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 to be used through the ply. This number must be an odd number.
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.