<!-- source-page: 411 -->

![](images/page-411_f182d9d1bb4059e42d61f4a6ce3234c8489f54130124191b530f6d49ef0dd382.jpg)

<details>
<summary>text_image</summary>

F6
8
F5
7
F2
5
6
F4
4
3
1
F3
2
F1
3
2
1
Stack direction
</details>

Stack direction = 1 from face 6 to face 4   
Stack direction = 2 from face 3 to face 5   
Stack direction = 3 from face 1 to face 2

![](images/page-411_857b3523f92c6fbf358921e07a4302139fe88d585a9a706b9ad786caed734af4.jpg)

<details>
<summary>text_image</summary>

6
F5
3
F4
4
F2
5
F3
1
F1
2
3
Stack direction
</details>

Stack direction = 3 from face 1 to face 2

Figure 29.6.1–5 Stack directions for SC6R and SC8R elements.

\*SHELL SECTION, STACK DIRECTION=n  
\*SHELL GENERAL SECTION, STACK DIRECTION=n

where n = 1, 2, or 3.

# Abaqus/CAE Usage:

Use the following option to define the stacking direction based on the element’s isoparametric directions if the continuum shell is defined using a composite layup:

Property module: Create Composite Layup: select Continuum Shell as the Element Type: Stacking Direction: Element direction 1, Element direction 2, or Element direction 3

Use the following option to define the stacking direction based on the element’s isoparametric directions if the continuum shell is defined using a composite shell section:

Assign→Material Orientation: select regions: Use Default Orientation or Other Method: Stacking Direction: Element isoparametric direction 1, Element isoparametric direction 2, or Element isoparametric direction 3

Defining the stacking and thickness direction based on an orientation definition

Alternatively, you can define the element stacking direction based on a local orientation definition. For shell elements the orientation definition defines an axis about which the local 1 and 2 material directions may be rotated. This axis also defines an approximate normal direction. The element stacking and thickness directions are defined to be the element isoparametric direction that is closest to this approximate normal (see Figure 29.6.1–6).

“The pinched cylinder problem,” Section 2.3.2 of the Abaqus Benchmarks Guide, and “LE3: Hemispherical shell with point loads,” Section 4.2.3 of the Abaqus Benchmarks Guide, illustrate the

<!-- source-page: 412 -->

![](images/page-412_f26ef5f307b2c10471adf59214781bb37d6e65dd686d54b0bc4151d0e46e1101.jpg)

<details>
<summary>text_image</summary>

Cohesive section, stack direction
based on cylor1
Local cylindrical orientation cylor1:
a = 0, 0, 0
b = 10, 0, 0
(10, 0, 0)
Abaqus selects the isoparametric direction ε₂ that is
closest to the 1st (i.e., x¹, or radial) axis, at the center.
Global
a
(0, 0, 0)
x
z
Y
X
x′
b
ε₃
x′
ε₂
ε₁
</details>

Figure 29.6.1–6 Example illustrating the use of a cylindrical system to define the stacking direction.

use of a cylindrical and spherical orientation system, respectively, to define the stack and thickness direction independent of nodal connectivity.

Input File Usage: Use one of the following options to define the element stacking direction based on a user-defined orientation:

\*SHELL SECTION, STACK DIRECTION=ORIENTATION, ORIENTATION=name   
\*SHELL GENERAL SECTION, STACK DIRECTION=ORIENTATION, ORIENTATION=name

Abaqus/CAE Usage: Use the following option to define the stacking direction based on a user-defined orientation if the continuum shell is defined using a composite layup:

Property module: Create Composite Layup: select Continuum Shell as the Element Type: Stacking Direction: Layup orientation

Use the following option to define the stacking direction based on a user-defined orientation if the continuum shell is defined using a composite shell section:

Assign→Material Orientation: select regions: Use Default Orientation or Other Method: Stacking Direction: Normal direction of material orientation

Verifying the element stack and thickness direction

You can verify the element stack and thickness direction visually in Abaqus/CAE by either contouring the element section thickness or plotting the material axis. Generally, the in-plane dimensions are significantly larger than the element thickness. By contouring the shell section thickness, output variable STH, you can easily verify that all elements are oriented appropriately and have the correct thickness.

<!-- source-page: 413 -->

If the element is oriented improperly, one of the in-plane dimensions will become the element section thickness, resulting in a discontinuous contour plot.

Alternatively, you can plot the material axis to verify that the 3-axis points in the desired normal direction. If the element is oriented improperly, one of the in-plane axes (either the 1- or 2-axis) would point in the normal direction.

# Numbering of section points through the shell thickness

The section points through the thickness of the shell are numbered consecutively, starting with point 1. For shell sections integrated during the analysis, section point 1 is exactly on the bottom surface of the shell if Simpson’s rule is used, and it is the point that is closest to the bottom surface if Gauss quadrature is used. For general shell sections, section point 1 is always on the bottom surface of the shell.

For a homogeneous section the total number of section points is defined by the number of integration points through the thickness. For shell sections integrated during the analysis, you can define the number of integration points through the thickness. The default is five for Simpson’s rule and three for Gauss quadrature. For general shell sections, output can be obtained at three section points.

For a composite section the total number of section points is defined by adding the number of integration points per layer for all of the layers. For shell sections integrated during the analysis, you can define the number of integration points per layer. The default is three for Simpson’s rule and two for Gauss quadrature. For general shell sections, the number of section points for output per layer is three.

# Default output points

In Abaqus/Standard the default output points through the thickness of a shell section are the points that are on the bottom and top surfaces of the shell section (for integration with Simpson’s rule) or the points that are closest to the bottom and top surfaces (for Gauss quadrature). For example, if five integration points are used through a single layer shell, output will be provided for section points 1 (bottom) and 5 (top).

In Abaqus/Explicit all section points through the thickness of a shell section are written to the results file for element output requests.

<!-- source-page: 414 -->

<!-- source-page: 415 -->

# 29.6.2 CHOOSING A SHELL ELEMENT

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

# References

• “Shell elements: overview,” Section 29.6.1   
• “Three-dimensional conventional shell element library,” Section 29.6.7   
• “Continuum shell element library,” Section 29.6.8   
• “Axisymmetric shell element library,” Section 29.6.9   
• “Axisymmetric shell elements with nonlinear, asymmetric deformation,” Section 29.6.10   
• “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 Abaqus/Standard shell element library includes:

• elements for three-dimensional shell geometries;   
• elements for axisymmetric geometries with axisymmetric deformation;   
• elements for axisymmetric geometries with general deformation that is symmetric about one plane;   
• elements for stress/displacement, heat transfer, and fully coupled temperature-displacement analysis;   
• general-purpose elements, as well as elements specifically suitable for the analysis of “thick” or “thin” shells;   
• general-purpose, three-dimensional, first-order elements that use reduced or full integration;   
• elements that account for finite membrane strain;   
• elements that use five degrees of freedom per node where possible, as well as elements that always use six degrees of freedom per node; and   
• continuum shell elements.

The Abaqus/Explicit shell element library includes:

• general-purpose three-dimensional elements to model “thick” or “thin” shells that account for finite membrane strains;   
• small-strain elements;   
• fully coupled temperature-displacement analysis elements;   
• an element for axisymmetric geometries with axisymmetric deformation; and   
• continuum shell elements.

<!-- source-page: 416 -->

The naming convention for shell elements depends on the element dimensionality.

# Three-dimensional shell elements

Three-dimensional shell elements in Abaqus are named as follows:

![](images/page-416_74a66d4913cfafdfb1eb02546c03667634f3bfe9f7152aadbfcd0f9cf43e2d53.jpg)

<details>
<summary>text_image</summary>

S 8 R 5 W
warping considered in small-strain formulation
in ABAQUS/Explicit (optional)
optional: 5 dof (5);
coupled temperature-displacement (T);
small-strain formulation in ABAQUS/Explicit (S)
reduced integration (optional)
number of nodes
conventional stress/displacement shell (S);
continuum stress/displacement shell (SC);
triangular stress/displacement thin shell (STRI);
heat transfer shell (DS)
</details>

For example, S4R is a 4-node, quadrilateral, stress/displacement shell element with reduced integration and a large-strain formulation; and SC8R is an 8-node, quadrilateral, first-order interpolation, stress/displacement continuum shell element with reduced integration.

# Axisymmetric shell elements

Axisymmetric shell elements in Abaqus are named as follows:

![](images/page-416_9dc8ac641424fedf8b6f744ef636e46b5635657ec584f8508d7b45aade125004.jpg)

<details>
<summary>text_image</summary>

S AX 2 T
Optional:
coupled temperature-displacement (T);
number of Fourier modes (1, 2, 3, or 4)
order of interpolation
axisymmetric (AX); axisymmetric with
nonlinear, asymmetric deformation (AXA)
stress/displacement shell (S);
heat transfer shell (DS)
</details>

For example, DSAX1 is an axisymmetric, heat transfer shell element with first-order interpolation.

<!-- source-page: 417 -->

# Conventional stress/displacement shell elements

The conventional stress/displacement shell elements in Abaqus can be used in three-dimensional or axisymmetric analysis. In Abaqus/Standard they use linear or quadratic interpolation and allow mechanical and/or thermal (uncoupled) loading; in Abaqus/Explicit they use linear interpolation and allow mechanical loading. These elements can be used in static or dynamic procedures. Some elements include the effect of transverse shear deformation and thickness change, while others do not. Some elements allow large rotations and finite membrane deformation, while others allow large rotations but small strains.

# Interpolation of temperature and field variables in stress/displacement shell elements

The value of temperatures at the integration locations in the surface of the shell used to compute the thermal stresses depends on whether first-order or second-order elements are used. An average temperature is used at the integration location in linear elements so that the thermal strain is constant throughout the shell surface. A linearly varying temperature distribution is used in higher-order shell elements. Field variables in stress/displacement shell elements are interpolated the same way as temperatures.

# Stress/displacement continuum shell elements

The stress/displacement continuum shell elements in Abaqus can be used in three-dimensional analysis. Continuum shells discretize an entire three-dimensional body, unlike conventional shells which discretize a reference surface (see “Shell elements: overview,” Section 29.6.1). These elements have displacement degrees of freedom only, use linear interpolation, and allow mechanical and/or thermal (uncoupled) loading for static and dynamic procedures. The continuum shell elements are general-purpose shells that allow finite membrane deformation and large rotations and, thus, are suitable for nonlinear geometric analysis. These elements include the effects of transverse shear deformation and thickness change.

Continuum shell elements employ first-order layer-wise composite theory, and estimate throughthickness section forces from the initial elastic moduli. Unlike conventional shells, continuum shell elements can be stacked to provide more refined through-thickness response. Stacking continuum shell elements allows for a richer transverse shear stress and force prediction.

Although continuum shell elements discretize a three-dimensional body, care should be taken to verify whether the overall deformation sustained by these elements is consistent with their layer-wise plane stress assumption; that is, the response is bending dominated and no significant thickness change is observed (i.e., approximately less than 10% thickness change). Otherwise, regular three-dimensional solid elements (“Three-dimensional solid element library,” Section 28.1.4) should be used. Furthermore, the thickness strain mode may yield a small stable time increment for thin continuum shell elements in Abaqus/Explicit (see “Shell section behavior,” Section 29.6.4).

# Coupled temperature-displacement continuum shell elements

The coupled temperature-displacement continuum shell elements in Abaqus have continuum shell geometry and use linear interpolation for the geometry and displacements. The temperature is

<!-- source-page: 418 -->

interpolated linearly as well. The thermal formulation is similar to that used for three-dimensional coupled temperature-displacement solid elements with reduced integration, for which the temperature variation is trilinear (see “Solid (continuum) elements,” Section 28.1.1). The temperatures at the section points through the thickness are interpolated linearly from the temperatures at the nodes.

# Heat transfer shell elements

These elements, available only in Abaqus/Standard and only with conventional shell element geometry, are intended to model heat transfer in shell-type structures. They provide the values of temperature at a number of points through the thickness at each shell node. This output can be input directly to the equivalent stress analysis shell element for sequentially coupled thermal-stress analysis (“Sequentially coupled thermal-stress analysis,” Section 16.1.2).

# Temperature variation through the shell thickness

The temperature variation is assumed to be piecewise quadratic through the thickness, while the interpolation on the reference surface of the shell is the same as that of the corresponding stress elements. For shell sections integrated during the analysis (“Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5) you can specify the number of section points used for cross-section integration and thickness-direction temperature interpolation at each node. Only Simpson’s rule can be used for integration through the shell thickness.

The temperature on the bottom surface of the shell (the surface in the negative direction along the shell normal—see “Defining the initial geometry of conventional shell elements,” Section 29.6.3) is degree of freedom 11. The temperature on the top surface is degree of freedom $1 0 + n _ { s }$ . A maximum of 20 temperature degrees of freedom can exist at a node. For a single-layer shell $n _ { s }$ is the total number of integration points used through the shell section. If a single section point is used for the cross-section integration, there is no temperature variation through the thickness of the shell and the temperature of the entire shell cross-section is degree of freedom 11. For a multi-layered shell the temperature at the top of each layer is the same as the temperature at the bottom of the next layer. Therefore,

$$
n _ {s} = 1 + \sum_ {l = 1} ^ {\mathrm{layers}} (n _ {l} - 1),
$$

where $n _ { l } \ ( n _ { l } > 1 )$ is the number of integration points used in layer l. If $n _ { l } { = } 1 , n _ { s }$ is equal to the number of composite layers. In this case, there is no temperature variation through the thickness of the shell, and the temperature of the entire composite is degree of freedom 11. The internal energy storage and heat conduction terms for shells are integrated in the same way as in the corresponding continuum elements (see “Solid (continuum) elements,” Section 28.1.1).

# Using shells in a thermal-stress analysis

To use the temperatures that are saved in the Abaqus/Standard results file directly as input to a thermalstress analysis, the mesh and the specification of the number of temperature points in the shell sections

<!-- source-page: 419 -->

must be the same in the heat transfer and the stress analysis models. In addition, multi-layered heat transfer shell elements must have the same number of integration points in each layer.

# Coupled temperature-displacement shell elements

The coupled temperature-displacement shell elements available in Abaqus have conventional shell element geometry and use linear or quadratic interpolation for the geometry and displacements. The temperature is interpolated linearly from the corner or end nodes; the lower-order temperature interpolation in quadratic shells is chosen to give the same interpolation order for thermal strain, which is proportional to temperature, as for total strain. All terms in the governing equations are integrated in the reference surface of the shell using a conventional Gauss scheme; Simpson’s rule is used to integrate through the shell thickness.

# Temperature variation through the shell thickness

The temperature variation through the shell thickness is assumed to be piecewise quadratic and is interpolated from temperatures at a series of points through the thickness of the shell at each node. The number of temperature values to be used at each node is determined by the number of integration points that you specify in the shell section definition (see “Defining the shell section integration” in “Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5). Up to a maximum of 20 temperature values are stored as degrees of freedom 11, 12, 13, etc. (up to degree of freedom 30) in a manner that is identical to that used for heat transfer shell elements (see “Heat transfer shell elements” above).

# “Thick” versus “thin” conventional shell elements

Abaqus includes general-purpose, conventional shell elements as well as conventional shell elements that are valid for thick and thin shell problems. See below for a discussion of what constitutes a “thick” or “thin” shell problem. This concept is relevant only for elements with displacement degrees of freedom.

The general-purpose, conventional shell elements provide robust and accurate solutions to most applications and will be used for most applications. However, in certain cases, for specific applications in Abaqus/Standard, enhanced performance may be obtained with the thin or thick conventional shell elements; for example, if only small strains occur and five degrees of freedom per node are desired.

The continuum shell elements can be used for any thickness; however, thin continuum shell elements may result in a small stable time increment in Abaqus/Explicit.

# General-purpose conventional shell elements

These elements allow transverse shear deformation. They use thick shell theory as the shell thickness increases and become discrete Kirchhoff thin shell elements as the thickness decreases; the transverse shear deformation becomes very small as the shell thickness decreases.

Element types S3/S3R, S3RS, S3RT, S4, S4R, S4RS, S4RSW, S4RT, SAX1, SAX2, SAX2T, SC6R, and SC8R are general-purpose shells.

<!-- source-page: 420 -->

# Thick conventional shell elements

In Abaqus/Standard thick shells are needed in cases where transverse shear flexibility is important and second-order interpolation is desired. When a shell is made of the same material throughout its thickness, this occurs when the thickness is more than about 1/15 of a characteristic length on the surface of the shell, such as the distance between supports for a static case or the wavelength of a significant natural mode in dynamic analysis.

Abaqus/Standard provides element types S8R and S8RT for use only in thick shell problems.

# Thin conventional shell elements

In Abaqus/Standard thin shells are needed in cases where transverse shear flexibility is negligible and the Kirchhoff constraint must be satisfied accurately (i.e., the shell normal remains orthogonal to the shell reference surface). For homogeneous shells this occurs when the thickness is less than about 1/15 of a characteristic length on the surface of the shell, such as the distance between supports or the wave length of a significant eigenmode. However, the thickness may be larger than 1/15 of the element length.

Abaqus/Standard has two types of thin shell elements: those that solve thin shell theory (the Kirchhoff constraint is satisfied analytically) and those that converge to thin shell theory as the thickness decreases (the Kirchhoff constraint is satisfied numerically).

• The element that solves thin shell theory is STRI3. STRI3 has six degrees of freedom at the nodes and is a flat, faceted element (initial curvature is ignored). If STRI3 is used to model a thick shell problem, the element will always predict a thin shell solution.   
• The elements that impose the Kirchhoff constraint numerically are S4R5, STRI65, S8R5, S9R5, SAXA1n, and SAXA2n. These elements should not be used for applications in which transverse shear deformation is important. If these elements are used to model a thick shell problem, the elements may predict inaccurate results.

# Finite-strain versus small-strain shell elements

Abaqus has both finite-strain and small-strain shell elements. This concept is relevant only for elements with displacement degrees of freedom.

# Finite-strain shell elements

Element types S3/S3R, S4, S4R, S4T, SAX1, SAX2, SAX2T, SAXA1n, and SAXA2n account for finite membrane strains and arbitrarily large rotations; therefore, they are suitable for large-strain analysis. The underlying formulation is described in “Axisymmetric shell elements,” Section 3.6.2 of the Abaqus Theory Guide; “Finite-strain shell element formulation,” Section 3.6.5 of the Abaqus Theory Guide; and “Axisymmetric shell element allowing asymmetric loading,” Section 3.6.7 of the Abaqus Theory Guide.

Continuum shell elements SC6R and SC8R account for finite membrane strains, arbitrary large rotation, and allow for changes in thickness, making them suitable for large-strain analysis. Computation of the change in thickness is based on the element nodal displacements, which in turn are computed from an effective elastic modulus defined at the beginning of an analysis.
