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
The Analytical Field toolset
and
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
The Analytical Field toolset
and
The Discrete Field toolset,
for more information.
- Choose Determine overall thickness from
geometry to have
Abaqus/CAE
calculate the offset from the thickness defined on the geometry. You must
choose From Geometry on the Offset
tabbed page.
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.
|