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.
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).
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.