<!-- source-page: 431 -->

# 29.6.4 SHELL SECTION BEHAVIOR

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

# References

• “Shell elements: overview,” Section 29.6.1   
• “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5   
• “Using a general shell section to define the section behavior,” Section 29.6.6   
• \*SHELL GENERAL SECTION   
• \*SHELL SECTION   
• “Creating homogeneous shell sections,” Section 12.13.6 of the Abaqus/CAE User’s Guide, in the HTML version of this guide   
• “Creating composite shell sections,” Section 12.13.7 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

# Overview

The shell section behavior:

• may or may not require numerical integration over the section;   
• can be linear or nonlinear; and   
• can be homogeneous or composed of layers of different material.

# 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,” Section 29.6.6). 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,” Section 29.6.5) allows the cross-sectional

<!-- source-page: 432 -->

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,” Section 29.6.5) 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,” Section 29.6.6) 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 smallstrain 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,” Section 3.6.8 of the Abaqus Theory Guide, and generally provides a reasonable estimate of the shear flexibility of the shell. It also provides

<!-- source-page: 433 -->

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 begining of the analysis based on initial elastic properties given in the model data. 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 nor is it relevant for element type STRI3. Although element type S4 has four integration points, the transverse shear calculation is assumed constant over the element. 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 will calculate the transverse shear stiffness values required in the element formulation. You can override these default values. The default shear stiffness values are not calculated in some cases if estimates of shear moduli are unavailable during the preprocessing stage of input; for example, when the material behavior is defined by user subroutine UMAT, UHYPEL, UHYPER, or VUMAT or, in Abaqus/Standard, when the section behavior is defined in UGENS. You must define the transverse shear stiffnesses in such cases.

# Transverse shear stiffness definition

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

$$
\bar {K} _ {\alpha \beta} ^ {t s} = f _ {p} K _ {\alpha \beta} ^ {t s},
$$

where

$\bar { K } _ { \alpha \beta } ^ { t s }$ are the components of the section shear stiffness $( \alpha , \beta = 1$ refer to the default surface directions on the shell, as defined in “Conventions,” Section 1.2.2, 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

$K _ { \alpha \beta } ^ { t s }$ is the actual shear stiffness of the section (calculated by Abaqus or user-defined).

You can specify all three shear stiffness terms $( K _ { 1 1 } ^ { t s } , K _ { 2 2 } ^ { t s }$ , and $K _ { 1 2 } ^ { t s } = K _ { 2 1 } ^ { t s } )$ ; 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 $K _ { \alpha \beta } ^ { t s }$ is obtained. For shell elements of type S4R5, S8R5,

<!-- source-page: 434 -->

S9R5, STRI65, or SAXAn the average of $K _ { 1 1 } ^ { t s }$ and $K _ { 2 2 } ^ { t s }$ is used and $K _ { 1 2 } ^ { t s }$ is ignored. The $K _ { \alpha \beta } ^ { t s }$ have units of force per length.

The dimensionless factor $f _ { p }$ is defined as

$$
f _ {p} = 1 / (1 + 0. 2 5 \times 1 0 ^ {- 4} \frac {A}{t ^ {2}}),
$$

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

$$
t = \sqrt {1 2 \frac {D _ {4 4} + D _ {5 5} + D _ {6 6}}{D _ {1 1} + D _ {2 2} + D _ {3 3}}}.
$$

If you do not specify the $K _ { \alpha \beta } ^ { t s }$ , they are calculated as follows. For laminated plates and sandwich constructions the $K _ { \alpha \beta } ^ { t s }$ 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 $K _ { 1 2 } ^ { t s }$ can be nonzero.

When a general shell section is used and the section stiffness is given directly, the $K _ { \alpha \beta } ^ { t s }$ are defined as

$$
K _ {1 1} ^ {t s} = K _ {2 2} ^ {t s} = \left(\frac {1}{6} (D _ {1 1} + D _ {2 2}) + \frac {1}{3} D _ {3 3}\right) Y, \quad K _ {1 2} ^ {t s} = 0,
$$

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 stiffness. The definition of an appropriate stiffness depends on the shell’s material composition and its lay-up; that is, how 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

$$
K _ {1 1} ^ {t s} = \frac {5}{6} G _ {1 3} t, \quad K _ {2 2} ^ {t s} = \frac {5}{6} G _ {2 3} t, \quad \text {and} \quad K _ {1 2} ^ {t s} = 0. 0.
$$

$G _ { 1 3 }$ and $G _ { 2 3 }$ 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 will be different from the value for homogeneous ones; see “Transverse shear stiffness in composite shells and offsets from the midsurface,” Section 3.6.8 of the Abaqus Theory Guide, for a discussion of how the effective shear stiffness for elastic materials is obtained in Abaqus.

<!-- source-page: 435 -->

Checking the validity of using shell theory

For linear elastic materials the slenderness ratio, $K _ { \alpha \alpha } l ^ { 2 } / D _ { ( \alpha + 3 ) ( \alpha + 3 ) }$ , where $\alpha { = } 1$ or 2 (no sum on ) 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

$$
\frac {K _ {\alpha \alpha} l ^ {2}}{D _ {(\alpha + 3) (\alpha + 3)}} > 1 0 0,
$$

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 $K _ { \alpha \alpha }$ and $D _ { ( \alpha + 3 ) ( \alpha + 3 ) }$ , you must run a data check analysis using a composite general shell section definition. The $K _ { \alpha \alpha }$ 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” in “Output,” Section 4.1.1). The $D _ { \alpha \beta }$ 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 smallstrain 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.

# 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 “Shell element overview,” Section 3.6.1 of the Abaqus Theory Guide). 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

<!-- source-page: 436 -->

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.

<!-- source-page: 437 -->

# 29.6.5 USING A SHELL SECTION INTEGRATED DURING THE ANALYSIS TO DEFINE THE SECTION BEHAVIOR

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

# References

• “Shell elements: overview,” Section 29.6.1   
• “Shell section behavior,” Section 29.6.4   
• \*DISTRIBUTION   
• \*HOURGLASS STIFFNESS   
• \*SHELL SECTION   
• \*TRANSVERSE SHEAR STIFFNESS   
• “Creating homogeneous shell sections,” Section 12.13.6 of the Abaqus/CAE User’s Guide   
• “Creating composite shell sections,” Section 12.13.7 of the Abaqus/CAE User’s Guide   
• Chapter 23, “Composite layups,” of the Abaqus/CAE User’s Guide

# Overview

A shell section integrated during the analysis:

• is used when numerical integration through the thickness of the shell is required; and   
• can be associated with linear or nonlinear material behavior.

# Defining a homogeneous shell section

To define a shell made of a single material, use a material definition (“Material data definition,” Section 21.1.2) to define the material properties of the section and associate these properties with the section definition. Optionally, you can refer to an orientation (“Orientations,” Section 2.2.5) to be associated with this material definition. A spatially varying local coordinate system defined with a distribution (“Distribution definition,” Section 2.8.1) can be assigned to the shell section definition. Linear or nonlinear material behavior can be associated with the section definition. However, if the material response is linear, the more economic approach is to use a general shell section (see “Using a general shell section to define the section behavior,” Section 29.6.6).

You specify the shell thickness and the number of integration points to be used through the shell section (see below). For continuum shell elements the specified shell thickness is used to estimate certain section properties, such as hourglass stiffness, which are later computed using the actual thickness computed from the element geometry.

You must associate the section properties with a region of your model.

If the orientation definition assigned to a shell section definition is defined with distributions, spatially varying local coordinate systems are applied to all shell elements associated with the shell

<!-- source-page: 438 -->

section. A default local coordinate system (as defined by the distributions) is applied to any shell element that is not specifically included in the associated distribution.

Input File Usage: \*SHELL SECTION, ELSET=name, MATERIAL=name, ORIENTATION=name

where the ELSET parameter refers to a set of shell elements.

Abaqus/CAE Usage: Property module:

Create Section: select Shell as the section Category and

Homogeneous as the section Type: Section integration: During

analysis; Basic: Material: name

Assign→Material Orientation: select regions

Assign→Section: select regions

# Defining a composite shell section

You can define a laminated (layered) shell made of one or more materials. You specify the thickness, the number of integration points (see below), the material, and the orientation (either as a reference to an orientation definition or as an angle measured relative to the overall orientation definition) 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 in which the layers are specified.

Optionally, you can specify an overall orientation definition for the layers of a composite shell. A spatially varying local coordinate system defined with a distribution (“Distribution definition,” Section 2.8.1) can be used to specify the overall orientation definition for the layers of a composite shell.

For continuum shell elements the thickness is determined from the element geometry and may vary through the model for a given section definition. Hence, the specified thicknesses 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. The thickness ratios for the layers need not be given in physical units, nor do the sum of the layer relative thicknesses need to add to one. The specified shell thickness is used to estimate certain section properties, such as hourglass stiffness, which are later computed using the actual thickness computed from the element geometry.

Spatially varying thicknesses can be specified on the layers of conventional shell elements using distributions (“Distribution definition,” Section 2.8.1). A distribution that is used to define layer thickness must have a default value. The default layer thickness is used by any shell element assigned to the shell section that is not specifically assigned a value in the distribution.

An example of a section with three layers and three section points per layer is shown in Figure 29.6.5–1.

The material name specified for each layer refers to a material definition (“Material data definition,” Section 21.1.2). The material behavior can be linear or nonlinear.

The orientation for each layer is specified by either the name of the orientation (“Orientations,” Section 2.2.5) associated with the layer or the orientation angle in degrees for the layer. Spatially varying orientation angles can be specified on a layer using distributions (“Distribution definition,” Section 2.8.1). Orientation angles, , are measured positive counterclockwise around the normal and relative to the overall section orientation. If either of the two local directions from the overall section orientation is

<!-- source-page: 439 -->

![](images/page-439_dc51ab91ac120e50f217e21791f5ef0bdb0abdec3cc502b46870bd25e677cc2f.jpg)

<details>
<summary>text_image</summary>

n, shell normal
9 ×
8 ×
7 ×
× 6
× 5
3 ×
2 ×
1 ×
Use default of 3 section points per layer (also define temperature degrees of freedom for heat transfer)
Layer 3 (material 1, orientation 3)
Layer 2 (material 2, orientation 2)
Layer 1 (material 1, orientation 1)
Layers 1 & 3 use the same material in different orientations
t₃
t₂
t₁
Specify 3 temperature values read per layer for stress analysis
</details>

Figure 29.6.5–1 Example of composite shell section definition.

not in the surface of the shell, is applied after the section orientation has been projected onto the shell surface. If you do not specify an overall section orientation, is measured relative to the default local shell directions (see “Conventions,” Section 1.2.2).

You must associate the section properties with a region of your model.

If the orientation definition assigned to a shell section definition is defined with distributions, spatially varying local coordinate systems are applied to all shell elements associated with the shell section. A default local coordinate system (as defined by the distributions) is applied to any shell element that is not specifically included in the associated distribution.

Unless your model is relatively simple, you will find it increasingly difficult to define your model using composite shell sections as you increase the number of layers and as you assign different sections to different regions. It can also be cumbersome to redefine the sections after you add new layers or remove or reposition existing layers. To manage a large number of layers in a typical composite model, you may want to use the composite layup functionality in Abaqus/CAE. For more information, see Chapter 23, “Composite layups,” of the Abaqus/CAE User’s Guide.

Input File Usage: \*SHELL SECTION, ELSET=name, COMPOSITE, ORIENTATION=name where the ELSET parameter refers to a set of shell elements.

Abaqus/CAE Usage: Abaqus/CAE uses a composite layup or a composite shell section to define the layers of a composite shell.

Use the following option for a composite layup:

Property module: Create Composite Layup: select Conventional Shell or Continuum Shell as the Element Type: Section integration: During analysis: specify orientations, regions, and materials

<!-- source-page: 440 -->

Use the following options for a composite shell section:

Property module:

Create Section: select Shell as the section Category and Composite as the section Type: Section integration: During analysis

Assign→Material Orientation: select regions

Assign→Section: select regions

# Defining the shell section integration

Simpson’s rule and Gauss quadrature are provided to calculate the cross-sectional behavior of a shell. You can specify the number of section points through the thickness of each layer and the integration method as described below. The default integration method is Simpson’s rule with five points for a homogeneous section and Simpson’s rule with three points in each layer for a composite section.

The three-point Simpson’s rule and the two-point Gauss quadrature are exact for linear problems. The default number of section points should be sufficient for routine thermal-stress calculations and nonlinear applications (such as predicting the response of an elastic-plastic shell up to limit load). For more severe thermal shock cases or for more complex nonlinear calculations involving strain reversals, more section points may be required; normally no more than nine section points (using Simpson’s rule) are required. Gaussian integration normally requires no more than five section points.

Gauss quadrature provides greater accuracy than Simpson’s rule when the same number of section points are used. Therefore, to obtain comparable levels of accuracy, Gauss quadrature requires fewer section points than Simpson’s rule does and, thus, requires less computational time and storage space.

# Using Simpson’s rule

By default, Simpson’s rule will be used for the shell section integration. The default number of section points is five for a homogeneous section and three in each layer for a composite section.

Simpson’s integration rule should be used if results output on the shell surfaces or transverse shear stress at the interface between two layers of a composite shell is required and must be used for heat transfer and coupled temperature-displacement shell elements.

Input File Usage: \*SHELL SECTION, SECTION INTEGRATION=SIMPSON

Abaqus/CAE Usage: Use the following option for a composite layup:

Property module: composite layup editor: Section integration: During analysis, Thickness integration rule: Simpson

Use the following option for a homogeneous or composite shell section:

Property module: shell section editor: Section integration: During analysis; Basic: Thickness integration rule: Simpson

# Using Gauss quadrature

If you use Gauss quadrature for the shell section integration, the default number of section points is three for a homogeneous section and two in each layer for a composite section.
