You can specify an offset value that is greater in magnitude than 0.5. However, this technique should be used with caution in regions of high curvature. The element’s area and all kinematic quantities are calculated relative to the reference surface, which may lead to a surface area integration error, affecting the stiffness and mass of the shell. In an Abaqus/Standard analysis a spatially varying offset can be defined for conventional shells using a distribution (“Distribution definition,” Section 2.8.1). 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. An offset to the shell’s top surface is illustrated in Figure 29.6.6–1. 

text_image

SPOS SNEG SPOS SNEG SNEG SPOS n n Mid surface

a) OFFSET= 0 Reference surface and midsurface are coincident b) OFFSET= −0.5 (SNEG) Reference surface is the bottom surface c) OFFSET= +0.5 (SPOS) Reference surface is the top surface Figure 29.6.6–1 Schematic of shell offset for an offset value of 0.5. A shell offset value can be specified only if a material definition is referenced or a composite shell section is defined. Input File Usage: Use the following option to specify a value for the shell offset: \*SHELL GENERAL SECTION, OFFSET=offset The OFFSET parameter accepts a value, a label (SPOS or SNEG), or in an Abaqus/Standard analysis the name of a distribution that is used to define a spatially varying offset. Specifying SPOS is equivalent to specifying a value of 0.5; specifying SNEG is equivalent to specifying a value of −0.5. Abaqus/CAE Usage: Use the following option for a composite layup: Property module: composite layup editor: Section integration: Before analysis; Offset: choose a reference surface, specify an offset, or select a scalar discrete field Use the following option for a shell section assignment: Property module: Assign→Section: select regions: Section: select a homogeneous or composite shell section: Definition: select a reference surface, specify an offset, or select a scalar discrete field # Defining a variable thickness for conventional shells using distributions You can define a spatially varying thickness for conventional shells using a distribution (“Distribution definition,” Section 2.8.1). The thickness of continuum shell elements is defined by the element geometry. For composite shells the total thickness is defined by the distribution, and the layer thicknesses you specify are scaled proportionally such that the sum of the layer thicknesses is equal to the total thickness (including spatially varying layer thicknesses defined with a distribution). 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. If the shell thickness is defined for a shell section with a distribution, nodal thicknesses cannot be used for that section definition. Input File Usage: Use the following option to define a spatially varying thickness: \*SHELL SECTION, SHELL THICKNESS=distribution name Abaqus/CAE Usage: Use the following option for a conventional shell composite layup: Property module: composite layup editor: Section integration: Before analysis; Shell Parameters: Shell thickness: Element distribution: select an analytical field or an element-based discrete field Use the following option for a homogeneous shell section: Property module: shell section editor: Section integration: Before analysis; Basic: Shell thickness: Element distribution: select an analytical field or an element-based discrete field Use the following option for a composite shell section: Property module: shell section editor: Section integration: Before analysis; Advanced: Shell thickness: Element distribution: select an analytical field or an element-based discrete field # Defining a variable nodal thickness for conventional shells You can define a conventional shell with continuously varying thickness by specifying the thickness of the shell at the nodes. This method can be used only if the section is defined in terms of material properties; it cannot be used if the section behavior is defined by specifying the equivalent section properties directly. For continuum shell elements a continuously varying thickness can be defined through the element nodal geometry; hence, the nodal thickness is not meaningful. If you indicate that the nodal thicknesses will be specified, for homogeneous shells any constant shell thickness you specify will be ignored, and the shell thickness will be interpolated from the nodes. The thickness must be defined at all nodes connected to the element. For composite shells the total thickness is interpolated from the nodes, and the layer thicknesses you specify are scaled proportionally such that the sum of the layer thicknesses is equal to the total thickness (including spatially varying layer thicknesses defined with a distribution). If the shell thickness is defined for a shell section with a distribution, nodal thicknesses cannot be used for that section definition. However, if nodal thicknesses are used, you can still use distributions to define spatially varying thicknesses on the layers of conventional shell elements. Input File Usage: Use both of the following options: \*NODAL THICKNESS \*SHELL GENERAL SECTION, NODAL THICKNESS Abaqus/CAE Usage: Use the following option for a conventional shell composite layup: Property module: composite layup editor: Section integration: Before analysis; Shell Parameters: Nodal distribution: select an analytical field or a node-based discrete field Use the following option for a homogeneous shell section: Property module: shell section editor: Section integration: Before analysis; Basic: Nodal distribution: select an analytical field or a node-based discrete field Use the following option for a composite shell section: Property module: shell section editor: Section integration: Before analysis; Advanced: Nodal distribution: select an analytical field or a node-based discrete field # Defining the Poisson strain in shell elements in the thickness direction Abaqus allows for a possible uniform change in the shell thickness in a geometrically nonlinear analysis (see “Change of shell thickness” in “Choosing a shell element,” Section 29.6.2). The Poisson’s strain is based on a fixed section Poisson’s ratio, either user specified or computed by Abaqus based on the elastic portion of the material definition. By default, Abaqus computes the Poisson’s strain using a fixed section Poisson’s ratio of 0.5. Input File Usage: Use the following option to specify a value for the effective Poisson’s ratio: \*SHELL GENERAL SECTION, POISSON= Use the following option to cause the shell thickness to change based on the initial elastic properties of the material: \*SHELL GENERAL SECTION, POISSON=ELASTIC Abaqus/CAE Usage: Use the following option for a composite layup: Property module: composite layup editor: Section integration: Before analysis; Shell Parameters: Section Poisson's ratio: Use analysis default or Specify value: $\nu _ { e f f }$ Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: Before analysis; Advanced: Section Poisson's ratio: Use analysis default or Specify value: $\nu _ { e f f }$ You cannot specify a shell thickness direction behavior based on the initial elastic material definition in Abaqus/CAE. # Defining the thickness modulus in continuum shell elements The thickness modulus is used in computing the stress in the thickness direction (see “Thickness direction stress in continuum shell elements” in “Choosing a shell element,” Section 29.6.2). Abaqus computes a thickness modulus value by default based on the elastic portion of the material definitions in the initial configuration. Alternatively, you can provide a value. If the material properties are unavailable during the preprocessing stage of input; for example, when the material behavior is defined by the fabric material model or user subroutine UMAT or VUMAT, you must specify the effective thickness modulus directly. Input File Usage: Use the following option to define an effective thickness modulus directly: \*SHELL GENERAL SECTION, THICKNESS $\mathrm { M O D U L U S } { = } { E _ { e f f } }$ Abaqus/CAE Usage: Use the following option for a composite layup: Property module: composite layup editor: Section integration: Before analysis; Shell Parameters: Thickness modulus $E _ { e f f }$ to specify the thickness properties directly Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: Before analysis; Advanced: Thickness modulus $E _ { e f f }$ to specify the thickness properties directly # Defining the transverse shear stiffness You can provide nondefault values of the transverse shear stiffness. You must specify the transverse shear stiffness for shear flexible shells in Abaqus/Standard if the section properties are specified in user subroutine UGENS. If you do not specify the transverse shear stiffness, it will be calculated as described in “Shell section behavior,” Section 29.6.4. Input File Usage: Use both of the following options: \*SHELL GENERAL SECTION \*TRANSVERSE SHEAR STIFFNESS Abaqus/CAE Usage: Use the following option for a composite layup: Property module: composite layup editor: Section integration: Before analysis; Shell Parameters: toggle on Specify transverse shear Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: Before analysis; Advanced: toggle on Specify transverse shear # Defining the initial section forces and moments You can define initial stresses (see “Defining initial stresses” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) for general shell sections that will be applied as initial section forces and moments. Initial conditions can be specified only for the membrane forces, the bending moments, and the twisting moment. Initial conditions cannot be prescribed for the transverse shear forces. # Specifying the order of accuracy in the Abaqus/Explicit shell element formulation In Abaqus/Explicit you can specify second-order accuracy in the shell element formulation. See “Section controls,” Section 27.1.4, for more information. Input File Usage: \*SHELL GENERAL SECTION, CONTROLS=name Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Element Controls # Specifying nondefault hourglass control parameters for reduced-integration shell elements You can specify a nondefault hourglass control formulation or scale factors for elements that use reduced integration. See “Section controls,” Section 27.1.4, for more information. In Abaqus/Standard the nondefault enhanced hourglass control formulation is available only for S4R and SC8R elements. In Abaqus/Standard you can modify the default values for hourglass control stiffness based on the default total stiffness approach for elements that use hourglass control and define a scaling factor for the stiffness associated with the drill degree of freedom (rotation about the surface normal) for elements that use six degrees of freedom at a node. No default values are available for hourglass control stiffness if the section properties are specified in user subroutine UGENS. Therefore, you must specify the hourglass control stiffness when UGENS is used to specify the section properties for reduced-integration elements. The stiffness associated with the drill degree of freedom is the average of the direct components of the transverse shear stiffness multiplied by a scaling factor. In most cases the default scaling factor is appropriate for constraining the drill rotation to follow the in-plane rotation of the element. If an additional scaling factor is defined, the additional scaling factor should not increase or decrease the drill stiffness by more than a factor of 100.0 for most typical applications. Usually, a scaling factor between 0.1 and 10.0 is appropriate. There are no hourglass stiffness factors or scale factors for hourglass stiffness for the nondefault enhanced hourglass control formulation. You can define the scale factor for the drill stiffness for the nondefault enhanced hourglass control formulation. Input File Usage: Use both of the following options to specify a nondefault hourglass control formulation or scale factors for reduced-integration elements: \*SECTION CONTROLS, NAME=name \*SHELL GENERAL SECTION, CONTROLS=name Use both of the following options in Abaqus/Standard to modify the default values for hourglass control stiffness based on the default total stiffness approach for reduced-integration elements and to define a scaling factor for the stiffness associated with the drill degree of freedom (rotation about the surface normal) for six degree of freedom elements: \*SHELL GENERAL SECTION \*HOURGLASS STIFFNESS Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Element Controls # Defining density for conventional shells You can define the mass per unit area for conventional shell elements whose section properties are specified directly in terms of the section stiffness (either directly in the section definition or, in Abaqus/Standard, in user subroutine UGENS). The density is required, for example, in a dynamic analysis or for gravity loading. See “Density,” Section 21.2.1, for details. The density is defined as part of the material definition for shells whose section properties include a material definition. This functionality is similar to the more general functionality of defining a nonstructural mass contribution (see “Nonstructural mass definition,” Section 2.7.1.) The only difference between the two definitions is that the nonstructural mass contributes to the rotary inertia terms about the midsurface while the additional mass defined in the section definition does not. Input File Usage: Use the following option to define the density directly: \*SHELL GENERAL SECTION, ELSET=name, DENSITY= Use the following option in Abaqus/Standard to define the density in user subroutine UGENS: \*SHELL GENERAL SECTION, ELSET=name, USER, DENSITY= Abaqus/CAE Usage: Use the following option for a composite layup: Property module: composite layup editor: Section integration: Before analysis; Shell Parameters: toggle on Density, and enter Use the following option for a homogeneous or composite shell section: Property module: shell section editor: Section integration: Before analysis; Advanced: toggle on Density, and enter You cannot define the shell section properties in user subroutine UGENS in Abaqus/CAE. # Defining damping You can include mass and stiffness proportional damping in a shell section definition. See “Material damping,” Section 26.1.1, for more information about material damping in Abaqus. # Specifying temperature and field variables Temperatures and field variables can be specified by defining the value at the reference surface of the shell or by defining the values at the nodes of a continuum shell element. The actual values of the temperatures and field variables are specified as either predefined fields or initial conditions (see “Predefined fields,” Section 34.6.1, or “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). # Output The following output variables are available from Abaqus/Explicit as element output: section forces and moments, section strains, element energies, element stable time increment, and element mass scaling factor. The output that is available from Abaqus/Standard depends on how the section behavior is defined. # Output if the section is defined in terms of material properties For shells whose section properties include a material definition (homogeneous or composite), section forces and moments and section strains are available as element output. The section moments are calculated relative to the reference surface. In addition, stress (in-plane and, for certain elements, transverse shear), strain, and orthotropic failure measures can be output. Since the behavior of the material is linear, three section points per layer (the bottom, middle, and top, respectively) are available for output. Stress invariants and principal stresses are not available as output but can be visualized in Abaqus/CAE. # Output if the equivalent section properties are specified directly or in UGENS If the matrix is used to specify the equivalent section properties directly or if user subroutine UGENS is used, section point stresses and strains and section strains are not available for output or visualization inAbaqus/CAE; only section forces and moments can be requested for outputor visualized inAbaqus/CAE. # 29.6.7 THREE-DIMENSIONAL CONVENTIONAL SHELL ELEMENT LIBRARY Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE # References • “Shell elements: overview,” Section 29.6.1 • “Choosing a shell element,” Section 29.6.2 • \*NODAL THICKNESS • \*SHELL GENERAL SECTION • \*SHELL SECTION # Overview This section provides a reference to the three-dimensional shell elements available in Abaqus/Standard and Abaqus/Explicit. # Element types Stress/displacement elements

$STRI3^{(S)}$	3-node triangular facet thin shell
S3	3-node triangular general-purpose shell, finite membrane strains (identical to element S3R)
S3R	3-node triangular general-purpose shell, finite membrane strains (identical to element S3)
$S3RS^{(E)}$	3-node triangular shell, small membrane strains
$STRI65^{(S)}$	6-node triangular thin shell, using five degrees of freedom per node
S4	4-node general-purpose shell, finite membrane strains
S4R	4-node general-purpose shell, reduced integration with hourglass control, finite membrane strains
$S4RS^{(E)}$	4-node, reduced integration, shell with hourglass control, small membrane strains
$S4RSW^{(E)}$	4-node, reduced integration, shell with hourglass control, small membrane strains, warping considered in small-strain formulation
$S4R5^{(S)}$	4-node thin shell, reduced integration with hourglass control, using five degrees of freedom per node
$S8R^{(S)}$	8-node doubly curved thick shell, reduced integration

S8R5(S) 8-node doubly curved thin shell, reduced integration, using five degrees of freedom per node S9R5(S) 9-node doubly curved thin shell, reduced integration, using five degrees of freedom per node # Active degrees of freedom 1, 2, 3, 4, 5, 6 for STRI3, S3R, S3RS, S4, S4R, S4RS, S4RSW, S8R 1, 2, 3 and two in-surface rotations for STRI65, S4R5, S8R5, S9R5 at most nodes 1, 2, 3, 4, 5, 6 for STRI65, S4R5, S8R5, S9R5 at any node that • has a boundary condition on a rotational degree of freedom; • is involved in a multi-point constraint that uses rotational degrees of freedom; • is attached to a beam or to a shell element that uses six degrees of freedom at all nodes (such as S4R, S8R, STRI3, etc.); • is a point where different elements have different surface normals (user-specified normal definitions or normal definitions created by Abaqus because the surface is folded); or • is loaded with moments. # Additional solution variables Element type S8R5 has three displacement and two rotation variables at an internally generated midbody node. # Heat transfer elements DS3(S) 3-node triangular shell DS4(S) 4-node quadrilateral shell DS6(S) 6-node triangular shell DS8(S) 8-node quadrilateral shell # Active degrees of freedom 11, 12, etc. (temperatures through the thickness as described in “Choosing a shell element,” Section 29.6.2) # Additional solution variables None. # Coupled temperature-displacement elements S3T(S) 3-node triangular general-purpose shell, finite membrane strains, bilinear temperature in the shell surface (identical to element S3RT) S3RT 3-node triangular general-purpose shell, finite membrane strains, bilinear temperature in the shell surface (for Abaqus/Standard it is identical to element S3T )