| Abaqus Keywords Reference Guide |
|
| How to find keyword examples |
| Abaqus Keywords Reference Guide |
|
| How to find keyword examples |
This option is used to specify a shell cross-section.
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE
Type: Model data
Level: Part, Part instance
Abaqus/CAE: Property module
Set this parameter equal to the name of the element set containing the shell elements for which the section behavior is being defined.
Include this parameter if the shell is made up of several layers of material.
Set this parameter equal to the name of the material of which the shell is made.
In an Abaqus/Explicit analysis, set this parameter equal to the name of a section controls definition (see “Section controls,” Section 27.1.4 of the Abaqus Analysis User's Guide) to be used to specify the second-order accurate element formulation option, a nondefault hourglass control formulation option, or scale factors.
In an Abaqus/Standard analysis, set this parameter equal to the name of a section controls definition to be used to specify the enhanced hourglass control formulation (see “Section controls,” Section 27.1.4 of the Abaqus Analysis User's Guide) or to be used in a subsequent Abaqus/Explicit import analysis.
Set this parameter equal to a mass per unit surface area of the shell.
If this parameter is used, the mass of the shell includes a contribution from this parameter in addition to any contribution from the material definition.
This parameter is relevant only when the COMPOSITE parameter is used.
Set this parameter equal to the name of a composite layup (see Chapter 23, “Composite layups,” of the Abaqus/CAE User's Guide). Abaqus/CAE uses this name to identify the composite layup that contains the shell section.
Include this parameter to indicate that the shell thickness should not be read from the data lines but should be interpolated from the thickness specified at the nodes with the *NODAL THICKNESS option. For composite sections the total thickness is interpolated from the nodes and the thicknesses of the layers specified on the data lines are scaled proportionally. This parameter is ignored for continuum shells.
The NODAL THICKNESS and SHELL THICKNESS parameters are mutually exclusive.
Include this parameter to define the distance (as a fraction of the shell thickness) from the shell midsurface to the reference surface (containing the nodes of the element). This parameter accepts positive or negative values, the labels SPOS or SNEG, or in an Abaqus/Standard analysis the name of a distribution. See “Distribution definition,” Section 2.8.1 of the Abaqus Analysis User's Guide.
Positive values of the offset are in the positive normal direction (see “Shell elements: overview,” Section 29.6.1 of the Abaqus Analysis User's Guide). When OFFSET=0.5 (or SPOS), the top surface of the shell is the reference surface. When OFFSET=–0.5 (or SNEG), the bottom surface of the shell is the reference surface. The default is OFFSET=0, which indicates that the middle surface of the shell is the reference surface.
In an Abaqus/Standard analysis a spatially varying offset can be specified by setting OFFSET equal to the name of a distribution. The distribution used to define the shell offset must have a default value. The default offset is used by any shell element assigned to the shell section that is not specifically assigned a value in the distribution.
Set this parameter equal to the name of an orientation definition (“Orientations,” Section 2.2.5 of the Abaqus Analysis User's Guide) to be used with material calculations in this definition of shell section behavior. This orientation will be used for material calculations and stress output in the individual layers, for the section forces output, and for the transverse shear stiffness.
It is possible to use a different orientation definition for material calculations in the individual layers of a composite shell by referencing an orientation definition or giving an orientation angle (in degrees, positive counterclockwise relative to the shell local directions) on each layer definition data line. Any layer definition line that does not have an orientation reference or an angle specified will use the orientation defined here. While an orientation defined with a distribution can be used to specify the overall orientation for the shell section, an orientation defined with a distribution cannot be specified on the layers of a composite shell.
Include this parameter to define the shell thickness direction behavior.
Set this parameter equal to a nonzero value to cause the thickness direction strain under plane stress conditions to be a linear function of the membrane strains. The value of the POISSON parameter must be between –1.0 and 0.5.
Set POISSON=ELASTIC to automatically select this parameter value based on the initial elastic part of the material definition.
Set POISSON=MATERIAL in an Abaqus/Explicit analysis to cause the thickness direction strain under plane stress conditions to be a function of the membrane strains and the in-plane material properties.
In Abaqus/Standard the default is POISSON=0.5; in Abaqus/Explicit the default is POISSON=MATERIAL.
Set SECTION INTEGRATION=SIMPSON (default) to use Simpson's rule for the shell section integration.
Set SECTION INTEGRATION=GAUSS to use Gauss quadrature for the shell section integration. Gauss quadrature cannot be used for heat transfer or thermally coupled shell elements.
Set this parameter equal to the name of a distribution (“Distribution definition,” Section 2.8.1 of the Abaqus Analysis User's Guide) to define spatially varying thickness. If this parameter is used for a non-composite section the thickness on the data line is ignored. For composite sections the total thickness is defined by the distribution and the thicknesses of the layers specified on the data lines are scaled proportionally. This parameter is ignored for continuum shells.
The distribution used to define shell thickness must have a default value. The default thickness is used by any shell element assigned to the shell section that is not specifically assigned a value in the distribution.
The NODAL THICKNESS and SHELL THICKNESS parameters are mutually exclusive.
This parameter is relevant only for continuum shells.
Set this parameter equal to 1, 2, 3, or ORIENTATION to define the continuum shell stack or thickness direction. Specify one of the numerical values to select the corresponding isoparametric direction of the element as the stack or thickness direction. The default is STACK DIRECTION=3.
If STACK DIRECTION=ORIENTATION, the ORIENTATION parameter is also required.
To obtain a desired thickness direction, the appropriate numerical value for the STACK DIRECTION parameter depends on the element connectivity. For a mesh-independent specification, use STACK DIRECTION=ORIENTATION. If the orientation assigned to the ORIENTATION parameter is defined with a distribution (“Distribution definition,” Section 2.8.1 of the Abaqus Analysis User's Guide), STACK DIRECTION=ORIENTATION is not supported.
This parameter is relevant only when the COMPOSITE parameter is used.
Include this parameter if the layers in the composite shell are symmetric about a central core. This parameter cannot be used if a spatially varying thickness or orientation angle is defined on any composite layer using a distribution (“Distribution definition,” Section 2.8.1 of the Abaqus Analysis User's Guide).
Use this parameter to select the mode of temperature and field variable input used on the *FIELD, the *INITIAL CONDITIONS, or the *TEMPERATURE options.
Omit the TEMPERATURE parameter to define the predefined field by its magnitude on the reference surface of the shell and its gradient through the thickness.
Set TEMPERATURE=n, where n (≥1) is the number of predefined field variable points in the shell or in each layer if the COMPOSITE parameter is used, to define the predefined field at n equally spaced points through each layer of the shell section.
In a heat transfer analysis step or a coupled temperature-displacement analysis step when the *FIELD option is used to specify values of predefined field variables, the TEMPERATURE parameter is required to specify the number of field variable points in the shell. The number of temperature points in the shell with temperature degrees of freedom is defined by the number of integration points specified on the data lines.
This parameter is relevant only for continuum shells.
Set this parameter equal to an effective thickness modulus. The default effective thickness modulus is twice the initial in-plane shear modulus based on the material definition.
First (and only) line:
Shell thickness. This value is ignored if the NODAL THICKNESS or SHELL THICKNESS parameters are included.
Number of integration points to be used through the shell section. The default is five points if Simpson's rule is used and three points if Gauss quadrature is used. The number of integration points must be an odd number for Simpson's rule and is equal to the number of temperature degrees of freedom at a node of the element if this section is associated with heat transfer or coupled temperature-displacement elements. The maximum number of points for Simpson's rule is 99, and in the case of heat transfer or coupled temperature-displacement elements it is 19. This number must be at least 2 and less than or equal to 15 for Gauss quadrature. For Simpson's rule it must be at least 3, except in a pure heat transfer analysis, where the number of integration points can be 1 for a constant temperature through the shell thickness.
First line:
For conventional shell elements enter a positive scalar value defining the actual layer thickness or the name of a distribution (“Distribution definition,” Section 2.8.1 of the Abaqus Analysis User's Guide) that defines spatially varying layer thicknesses. The layer thickness is modified if the NODAL THICKNESS or SHELL THICKNESS parameter is included.
For continuum shell elements enter a positive scalar value defining the relative thickness of this layer with respect to the other layers. The thickness ratios for the layers need not be given in physical units, nor is it required that the layer relative thicknesses add to one.
Number of integration points to be used through the layer. The default is three points if Simpson's rule is used and two points if Gauss quadrature is used. The number of integration points must be an odd number for Simpson's rule, and it determines the number of temperature degrees of freedom at a node of the element if this section is associated with heat transfer or coupled temperature-displacement elements. The maximum number of points for Simpson's rule is 99, and in the case of heat transfer or coupled temperature-displacement elements it is 19. This number must be less than or equal to 15 for Gauss quadrature.
Name of the material forming this layer.
Name of the orientation to be used with this layer, an orientation angle, 
, or the name of a distribution (“Distribution definition,” Section 2.8.1 of the Abaqus Analysis User's Guide) that defines spatially varying orientation angles. If the name of an orientation is used, the orientation cannot be defined with distributions. Orientation angles (in degrees) are measured positive counterclockwise relative to the orientation definition given with the ORIENTATION parameter. If the ORIENTATION parameter is not included, is measured relative to the default shell local directions (see “Orientations,” Section 2.2.5 of the Abaqus Analysis User's Guide).
Name of the ply. Required only for composite layups defined in Abaqus/CAE. You must specify ply names that are unique throughout the entire model to ensure the correct display of ply-based results.
Repeat this data line as often as necessary. Use one data line for each layer of the shell. The order of the laminated shell layers with respect to the positive direction of the shell normal is defined by the order of the data lines. If the SYMMETRIC parameter is included, specify only half the layers, from the bottom layer to the midplane.