Shell Section Behavior

Methods for Defining the Shell Section Behavior

Two methods are provided to define the cross-sectional behavior of a shell.

Linear moment-bending and force-membrane strain relationships can be defined by using a general shell section (see Using a General Shell Section to Define the Section Behavior). In this case all calculations are done in terms of section forces and moments.

In Abaqus/Standard when section properties are given directly (i.e., the section is not associated with one or more material definitions), strains and stresses are not available for output. However, when section properties are specified by one or more elastic material layers, strains and stresses are available when requested for output. In Abaqus/Explicit stresses and strains are not available for output at the section points whenever a general shell section is used; only section forces, section moments, and section strains are available for output.

In Abaqus/Standard nonlinear behavior of the shell section, formulated in terms of forces and moments, can be defined by using a general shell section in conjunction with user subroutine UGENS.
Alternatively, a shell section integrated during the analysis (see Using a Shell Section Integrated during the Analysis to Define the Section Behavior) allows the cross-sectional behavior to be calculated by numerical integration through the shell thickness, thus providing complete generality in material modeling. With this type of section any number of material points can be defined through the thickness and the material response can vary from point to point.

Both general shell sections and shell sections integrated during the analysis allow layers of different materials, in different orientations, to be used through the cross-section. In these cases the section definition provides the shell thickness, material, and orientation per layer.

For conventional shell elements you can specify an offset of the reference surface from the shell's midsurface when the section properties are specified by one or more material layers. When the section properties are given directly, you cannot directly specify an offset; however, an offset can be included implicitly in the section properties. A nonzero offset cannot be specified for continuum shell elements. If a nonzero offset is specified for a continuum shell element, an error message is issued during input file preprocessing.

Determining Whether to Use a Shell Section Integrated during the Analysis or a General Shell Section

When a shell section integrated during the analysis (see Using a Shell Section Integrated during the Analysis to Define the Section Behavior) is used, Abaqus uses numerical integration through the thickness of the shell to calculate the section properties. This type of shell section is generally used with nonlinear material behavior in the section. It must be used with shells that provide for heat transfer, since general shell sections do not allow the definition of heat transfer properties.

Use a general shell section (see Using a General Shell Section to Define the Section Behavior) if the response of the shell is linear elastic and its behavior is not dependent on changes in temperature or predefined field variables or, in Abaqus/Standard, if nonlinear behavior in terms of forces and moments is to be defined in user subroutine UGENS.

Transverse Shear Stiffness

For all shell elements in Abaqus/Standard that use transverse shear stiffness and for the finite-strain shell elements in Abaqus/Explicit, the transverse shear stiffness is computed by matching the shear response for the shell to that of a three-dimensional solid for the case of bending about one axis. For the small-strain shell elements in Abaqus/Explicit the transverse shear stiffness is based on the effective shear modulus.

Transverse Shear Stiffness for Shell Elements in Abaqus/Standard and Finite-Strain Shell Elements in Abaqus/Explicit

In all shell elements in Abaqus/Standard that are valid for thick shell problems or that enforce the Kirchhoff constraint numerically (i.e., all shell elements except STRI3) and in the finite-strain shell elements in Abaqus/Explicit (S3R, S4, S4R, SAX1, SC6R, and SC8R), Abaqus computes the transverse shear stiffness by matching the shear response for the case of the shell bending about one axis, using a parabolic variation of transverse shear stress in each layer. The approach is described in Transverse shear stiffness in composite shells and offsets from the midsurface and generally provides a reasonable estimate of the shear flexibility of the shell. It also provides estimates of interlaminar shear stresses in composite shells. In calculating the transverse shear stiffness, Abaqus assumes that the shell section directions are the principal bending directions (bending about one principal direction does not require a restraining moment about the other direction). For composite shells with orthotropic layers that are not symmetric about the shell midsurface, the shell section directions may not be the principal bending directions. In such cases the transverse shear stiffness is a less accurate approximation and will change if different shell section directions are used. Abaqus computes the transverse shear stiffness only once at the beginning of the analysis based on initial elastic properties given in the model data. Initial temperature and field variable dependencies are considered. Any changes to the transverse shear stiffness that occur due to changes in the material stiffness during the analysis are ignored.

Axisymmetric shell elements SAX1 and SAX2; three-dimensional shell elements S3/S3R, S4, S4R, S8R, and S8RT; and continuum shell elements SC6R and SC8R are based on a first-order shear deformation theory. Other shell elements—such as S4R5, S8R5, S9R5, STRI65, and SAXAmn—use the transverse shear stiffness to enforce the Kirchhoff constraints numerically in the thin shell limit. The transverse shear stiffness is not relevant for shells without displacement degrees of freedom and is relevant only for element type STRI3 as part of a penalty term used to control drill rotations. Although element type S4 has four integration points, the transverse shear calculation is assumed constant over the element. A higher resolution of the transverse shear may be obtained by stacking continuum shell elements.

For most shell sections, including layered composite or sandwich shell sections, Abaqus calculates the transverse shear stiffness values required in the element formulation. You can override these default values (see Defining the Transverse Shear Stiffness for shell sections and Defining the Transverse Shear Stiffness for general shell sections). In some cases the default shear stiffness values are not calculated if estimates of the shear moduli are unavailable during the preprocessing stage of input; for example, when the section behavior is defined in user subroutine UGENS in Abaqus/Standard. You must define the transverse shear stiffnesses in such cases. When a shell section's material behavior is defined by a user subroutine (for example, UMAT, UHYPEL, UHYPER, or VUMAT), you must define the transverse shear modulus for the material (see Defining the Elastic Transverse Shear Modulus) or the transverse shear stiffness for the section.

Transverse Shear Stiffness Definition

The transverse shear stiffness of the section of a shear flexible shell element is defined in Abaqus as

{\bar{K}}_{α β}^{t s} = f_{p} K_{α β}^{t s},

where

${\bar{K}}_{α β}^{t s}$: are the components of the section shear stiffness ( $α, β = 1, 2$ refer to the default surface directions on the shell, as defined in Conventions, or to the local directions associated with the shell section definition);
$f_{p}$: is a dimensionless factor that is used to prevent the shear stiffness from becoming too large in thin shells; and
$K_{α β}^{t s}$: is the actual shear stiffness of the section (calculated by Abaqus or user-defined).

You can specify all three shear stiffness terms ( $K_{11}^{t s}$ , $K_{22}^{t s}$ , and $K_{12}^{t s} = K_{21}^{t s}$ ); otherwise, they will take the default values defined below. The dimensionless factor $f_{p}$ is always included in the calculation of transverse shear stiffness, regardless of the way $K_{α β}^{t s}$ is obtained. For shell elements of type S4R5, S8R5, S9R5, STRI65, or SAXAn the average of $K_{11}^{t s}$ and $K_{22}^{t s}$ is used and $K_{12}^{t s}$ is ignored. The $K_{α β}^{t s}$ have units of force per length.

The dimensionless factor $f_{p}$ is defined as

f_{p} = 1 / (1 + 0.25 \times 10^{- 4} \frac{A}{t^{2}}),

where A is the area of the element and t is the thickness of the shell. When a general shell section definition not associated with one or more material definitions is used to define the shell section stiffness, the thickness of the shell, t, is estimated as

t = \sqrt{12 \frac{D_{44} + D_{55} + D_{66}}{D_{11} + D_{22} + D_{33}}} .

If you do not specify the $K_{α β}^{t s}$ , they are calculated as follows. For laminated plates and sandwich constructions the $K_{α β}^{t s}$ are estimated by matching the elastic strain energy associated with shear deformation of the shell section with that based on piecewise quadratic variation of the transverse shear stress across the section, under conditions of bending about one axis. For unsymmetric lay-ups the coupling term $K_{12}^{t s}$ can be nonzero.

When a general shell section is used and the section stiffness is given directly, the $K_{α β}^{t s}$ are defined as

K_{11}^{t s} = K_{22}^{t s} = (\frac{1}{6} (D_{11} + D_{22}) + \frac{1}{3} D_{33}) Y, K_{12}^{t s} = 0,

where $D_{i j}$ is the section stiffness matrix and Y is the initial scaling modulus.

When a user subroutine (for example, UMAT, UHYPEL, UHYPER, or VUMAT) is used to define a shell element's material response, you must define the transverse shear modulus for the material or the transverse shear stiffness for the shell. The definition of an appropriate stiffness depends on the shell's material composition and its lay-up; that is, how the material is distributed through the thickness of the cross-section.

The transverse shear stiffness should be specified as the initial, linear elastic stiffness of the shell in response to pure transverse shear strains. For a homogeneous shell made of a linear, orthotropic elastic material, where the strong material direction aligns with the element's local 1-direction, the transverse shear stiffness should be

K_{11}^{t s} = \frac{5}{6} G_{13} t, K_{22}^{t s} = \frac{5}{6} G_{23} t, and K_{12}^{t s} = 0.0 .

$G_{13}$ and $G_{23}$ are the material's shear moduli in the out-of-plane direction. The number 5/6 is the shear correction coefficient that results from matching the transverse shear energy to that for a three-dimensional structure in pure bending. For composite shells the shear correction coefficient is different from the value for homogeneous ones; see Transverse shear stiffness in composite shells and offsets from the midsurface for a discussion of how the effective shear stiffness for elastic materials is obtained in Abaqus.

Checking the Validity of Using Shell Theory

For linear elastic materials the slenderness ratio, $K_{α α} l^{2} / D_{(α + 3) (α + 3)}$ , where $α$ =1 or 2 (no sum on $α$ ) and l is a characteristic length on the surface of the shell, can be used as a guideline to decide if the assumption that plane sections must remain plane is satisfied and, hence, shell theory is adequate. Generally, if

\frac{K_{α α} l^{2}}{D_{(α + 3) (α + 3)}} > 100,

shell theory will be adequate; for smaller values the membrane strains will not vary linearly through the section, and shell theory will probably not give sufficiently accurate results. The characteristic length, l, is independent of the element length and should not be confused with the element's characteristic length, $L_{c}$ .

To obtain the $K_{α α}$ and $D_{(α + 3) (α + 3)}$ , you must run a data check analysis using a composite general shell section definition. The $K_{α α}$ will be printed under the title “TRANSVERSE SHEAR STIFFNESS FOR THE SECTION” in the data (.dat) file if you request model definition data (see Controlling the Amount of analysis input file processor Information Written to the Data File). The $D_{α β}$ will be printed out under the title “SECTION STIFFNESS MATRIX.”

Transverse Shear Stiffness for Small-Strain Shell Elements in Abaqus/Explicit

When a shell section integrated during the analysis is used, the transverse shear stresses for the small-strain shells in Abaqus/Explicit are assumed to have a piecewise constant distribution in each layer. The transverse shear force will converge to the correct solution for single or multilayer isotropic sections and single-layer orthotropic sections. The transverse shear stiffness is approximate for multilayer orthotropic sections where convergence to the proper transverse shear behavior may not be obtained as shells become thick and principal material directions deviate from the principal section directions. The finite-strain S4R element should be used with a shell section integrated during the analysis if accurate through-thickness transverse shear stress distributions are required for the analysis of composite shells.

The same transverse shear stiffness described for the finite-strain shells is used to calculate the transverse shear force for the small-strain shells in Abaqus/Explicit when a general shell section is used. Thus, for this case the transverse shear force for multilayer composite shells will converge to the correct value for both thin and thick sections.

Drill Stiffness and Transverse Shear

Shell elements in Abaqus use a small penalty stiffness to control drill rotations. When used, the drill stiffness is proportional to the transverse shear stiffness. Drill stiffness is not needed for a five degree-of-freedom shell element unless three global rotation components are active on the element.

Bending Strain Measures

Most three-dimensional shell elements in Abaqus use bending strain measures that are approximations to those of Koiter-Sanders shell theory (see About the Abaqus shell element library). As per the Koiter-Sanders theory the displacement field normal to the shell surface does not produce any bending moments. For example, a purely radial expansion of a cylinder will result in only membrane stresses and strains—there are no variations through the thickness and, hence, no bending. This applies to both the incremental strain measures for linear elastic materials and the deformation gradient for hyperelastic materials. The only exception is for axisymmetric shell elements modeled with hyperelastic materials in Abaqus/Standard. In this case a variation of the membrane stresses and strains through the thickness can occur.

Nodal Mass and Rotary Inertia for Composite Sections

For composite shell sections Abaqus computes the nodal masses based on an average density through the section, weighted with respect to the layer thicknesses. This average density is used to compute an average rotary inertia as if the section were homogeneous. As a consequence, Abaqus does not account for an unsymmetric distribution of mass: the center of mass is assumed to be at the reference surface of the shell. For continuum shells the mass is equally distributed to the top and bottom surface nodes.