<!-- source-page: 451 -->

![](images/page-451_112e3e9179005051a324766d10fc680488b777f428d6d2e87ba144a459dbbec3.jpg)

<details>
<summary>text_image</summary>

composite shell section
n
layer 3
6 x
5 x
layer 2
x 4
x 3
layer 1
2 x
1 x
Use default of 2 section
points per layer
Specify 3 temperature points per layer,
shared at layer intersections,
7 total
n_T = 3
n_l = 3
1 + n_l (n_T - 1) = 7
</details>

Figure 29.6.5–4 Defining temperature values at n equally spaced points using Gauss integration.

In Abaqus/Explicit since no thermal MPCs and no thermal equation constraints are available for degrees of freedom greater than 11, care must be taken when using a different number of temperature points in adjacent shell elements. This should usually have a localized effect on the temperature distribution, but it may affect the overall solution for the cases in which the temperature gradient through the thickness is significant.

In both Abaqus/Standard and Abaqus/Explicit be careful in the models in which the shell’s normals are reversed. In this case the temperature at the bottom of the shell becomes the temperature at the top of the adjacent shell. This may have a small impact on the overall solution for the cases in which the thermal gradient through the thickness is negligible and the temperature variation is mainly in plane. However, if the temperature gradient through the thickness is significant, it may lead to incorrect results.

# Output

In an Abaqus/Standard stress analysis temperature output at the section points can be obtained using the element variable TEMP.

If the temperature values were specified at equally spaced points through the thickness, output at the temperature points can be obtained in an Abaqus/Standard stress analysis, as in a heat transfer analysis,

<!-- source-page: 452 -->

by using the nodal variable NTxx. This nodal output variable is also available in Abaqus/Explicit for coupled temperature-displacement analyses. The nodal variable NTxx should not be used for output at the temperature points with the default gradient method. In this case output variable NT should be requested; NT11 (the reference temperature value) and NT12 (the temperature gradient) will be output automatically. For continuum shell elements, there is only NT11; all other NTxx are irrelevant.

Other output variables that are relevant for shells are listed in each of the library sections describing the specific shell elements. For example, stresses, strains, section forces and moments, average section stresses, section strains, etc. can be output. The section moments are calculated relative to the reference surface.

<!-- source-page: 453 -->

# 29.6.6 USING A GENERAL SHELL SECTION 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   
• “UGENS,” Section 1.1.38 of the Abaqus User Subroutines Reference Guide   
• \*DISTRIBUTION   
• \*HOURGLASS STIFFNESS   
• \*SHELL GENERAL SECTION   
• \*TRANSVERSE SHEAR STIFFNESS   
• “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   
• “Creating general shell stiffness sections,” Section 12.13.10 of the Abaqus/CAE User’s Guide, in the HTML version of this guide   
• Chapter 23, “Composite layups,” of the Abaqus/CAE User’s Guide

# Overview

# A general shell section:

• is used when numerical integration through the thickness of the shell is not required;   
• can be associated with linear elastic material behavior or, in Abaqus/Standard, can invoke user subroutine UGENS to define nonlinear section properties in terms of forces and moments;   
• can be used to model an equivalent shell section for some more complex geometry (for example, replacing a corrugated shell with an equivalent smooth plate for global analysis); and   
• cannot be used with heat transfer and coupled temperature-displacement shells.

# Defining the shell section behavior

# A general shell section can be defined as follows:

• The section response can be specified by associating the section with a material definition or, in the case of a composite shell, with several different material definitions.   
• The section properties can be specified directly.   
• In Abaqus/Standard the section response can be programmed in user subroutine UGENS.

<!-- source-page: 454 -->

# Specifying the equivalent section properties by defining the layers (thickness, material, and orientation)

You can define the shell section’s mechanical response by specifying the thickness; the material reference; and the orientation of the section or, for a composite shell, the orientation of each of its layers. Abaqus will determine the equivalent section properties. You must associate the section behavior with a region of your model.

The linear elastic material behavior is defined with a material definition (“Material data definition,” Section 21.1.2), which may contain linear elastic behavior (“Linear elastic behavior,” Section 22.2.1) and thermal expansion behavior (“Thermal expansion,” Section 26.1.2). The density (“Density,” Section 21.2.1) and damping (“Material damping,” Section 26.1.1) behavior can also be specified as described below; in Abaqus/Explicit the density of the material must be defined. However, no nonlinear material properties, such as plastic behavior, can be included since Abaqus will precompute the section response and will not update that response during the analysis. Dependence of the linear elastic material behavior on temperature or predefined field variables is not allowed.

The shell section response is defined by

$$
\left\{\mathbf {N} \right\} = \left[ \mathbf {D} \right]: \left\{\mathbf {E} \right\} - \left\{\mathbf {N} ^ {\mathrm{th}} \right\}.
$$

No temperature-dependent scaling of the modulus is included. The section forces and moments caused by thermal strains, $\{ \mathbf { N } ^ { \mathbf { t h } } \}$ , vary linearly with temperature and are defined by

$$
\{\mathbf {N} ^ {\mathbf {t h}} \} = (\theta - \theta^ {I}) \{\bar {\mathbf {F}} \},
$$

where $\{ \bar { \bf F } \}$ are the generalized stresses caused by a fully constrained unit temperature rise that result from the user-defined thermal expansion, is the temperature, and $\theta ^ { I }$ is the initial (stress-free) temperature at this point in the shell (defined by the initial nodal temperatures given as initial conditions; see “Defining initial temperatures” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1).

# Defining a shell made of a single linear elastic material

To define a shell made of a single linear elastic material, you refer to the name of a material definition (“Material data definition,” Section 21.1.2) as described above. Optionally, you can define an orientation definition to be used with the section (“Orientations,” Section 2.2.5). A spatially varying local coordinate system defined with a distribution (“Distribution definition,” Section 2.8.1) can be assigned to the shell section definition. In addition, you specify the shell thickness as part of the section definition. For continuum shell elements the specified thickness is used to estimate certain section properties, such as hourglass stiffness, that are later computed from the element geometry.

You must associate this section behavior with a region of your model.

You can redefine the thickness, offset, section stiffness, and material orientation specified in the section definition on an element-by-element basis. See “Distribution definition,” Section 2.8.1.

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: 455 -->

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 GENERAL 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: Before analysis;

Basic: Material: name

Assign→Material Orientation: select regions

Assign→Section: select regions

# Defining a shell made of layers with different linear elastic material behaviors

You can define a shell made of layers with different linear elastic material behaviors. Optionally, you can define an orientation definition to be used with the section (“Orientations,” Section 2.2.5). A spatially varying local coordinate system defined with a distribution (“Distribution definition,” Section 2.8.1) can be assigned to the shell section definition.

You specify the layer thickness; the name of the material forming this layer (as described above); and the orientation angle, , (in degrees) measured positive counterclockwise relative to the specified section orientation definition. Spatially varying orientation angles can be specified on a layer using distributions (“Distribution definition,” Section 2.8.1). If either of the two local directions from the specified section orientation is 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 a section orientation, is measured relative to the default shell local directions (see “Conventions,” Section 1.2.2). 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.

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, that are later computed from the element geometry.

Spatially varying thicknesses can be specified on the layers of conventional shell elements (not continuum 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.

You must associate this section behavior 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.

<!-- source-page: 456 -->

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 GENERAL 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 a shell made of layers with different linear elastic material behaviors.

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: Before analysis: specify orientations, regions, and materials

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: Before analysis

Assign→Material Orientation: select regions

Assign→Section: select regions

# Specifying the equivalent section properties directly for conventional shells

You can define the section’s mechanical response by specifying the general section stiffness and thermal expansion response— , , $Y ( \theta , f _ { \beta } )$ and $\alpha ( \theta , f _ { \beta } )$ , as defined below—directly. Since this method then provides the complete specification of the section’s mechanical response, no material reference is needed. Optionally, you can define $\theta ^ { 0 }$ , the reference temperature for thermal expansion.

You must associate this section behavior with a region of your model.

In this case the shell section response is defined by

$$
\{\mathbf {N} \} = Y (\theta , f _ {\beta}) [ \mathbf {D} ]: \{\mathbf {E} \} - \{\mathbf {N} ^ {\mathbf {t h}} \},
$$

where

{N} are the forces and moments on the shell section (membrane forces per unit length, bending moments per unit length);

are the generalized section strains in the shell (reference surface strains and curvatures);

[D] is the section stiffness matrix;

$Y ( \theta , f _ { \beta } )$ is a scaling modulus, which can be used to introduce temperature and field-variable $\left( f _ { \beta } \right)$ dependence of the cross-section stiffness; and

<!-- source-page: 457 -->

$\{ \mathbf { N } ^ { \mathbf { t h } } \}$ are the section forces and moments (per unit length) caused by thermal strains.

These thermal forces and moments in the shell are generated according to the formula

$$
\left\{\mathbf {N} ^ {\mathbf {t h}} \right\} = \left(\alpha \left(\theta , f _ {\beta}\right) \left(\theta - \theta^ {0}\right) - \alpha \left(\theta^ {I}, f _ {\beta} ^ {I}\right) \left(\theta^ {I} - \theta^ {0}\right)\right) \left\{\mathbf {F} \right\},
$$

where

$\alpha ( \theta , f _ { \beta } )$ is a scaling factor (the “thermal expansion coefficient”);

$\theta ^ { I }$ is the initial (stress-free) temperature at this point in the shell, defined by the initial nodal temperatures given as initial conditions (“Defining initial temperatures” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1); and

{F} are the user-specified generalized section forces and moments (per unit length) caused by a fully constrained unit temperature rise.

If the coefficient of thermal expansion, , is not a function of temperature, the value of $\theta ^ { 0 }$ is not needed. Note the distinction between $\theta ^ { 0 }$ , the reference value used in defining , and the stress-free initial temperature, $\theta ^ { I }$ .

In these equations the order of the terms is

$$
\{\mathbf {N} \} = \left\{ \begin{array}{l} N _ {1 1} \\ N _ {2 2} \\ N _ {1 2} \\ M _ {1 1} \\ M _ {2 2} \\ M _ {1 2} \end{array} \right\}, \qquad \{\mathbf {E} \} = \left\{ \begin{array}{l} \varepsilon_ {1 1} \\ \varepsilon_ {2 2} \\ \gamma_ {1 2} \\ \kappa_ {1 1} \\ \kappa_ {2 2} \\ \kappa_ {1 2} \end{array} \right\};
$$

that is, the direct membrane terms come first, then the shear membrane term, then the direct and shear bending terms, with six terms in all. Engineering measures of shear membrane strain $( \gamma _ { 1 2 } )$ and twist ( ) are used in Abaqus.

This method of defining the shell section properties cannot be used with variable thickness shells or continuum shell elements.

See “Laminated composite shells: buckling of a cylindrical panel with a circular hole,” Section 1.2.2 of the Abaqus Example Problems Guide, for more information.

The stiffness matrix, , can be defined as a constant stiffness for the section or as a spatially varying stiffness by referring to a distribution (“Distribution definition,” Section 2.8.1). If a spatially varying stiffness is used, the distribution must have a default stiffness defined. The default stiffness is used by any shell element assigned to the shell section that is not specifically assigned a value in the distribution.

Input File Usage: \*SHELL GENERAL SECTION, ELSET=name, ZERO=

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

<!-- source-page: 458 -->

Abaqus/CAE Usage: Property module:

Create Section: select Shell as the section Category and General

shell stiffness as the section Type

Assign→Section: select regions

# Specifying the section properties in user subroutine UGENS

In Abaqus/Standard you can define the section response in user subroutine UGENS for the more general case where the section response may be nonlinear. User subroutine UGENS is particularly useful if the nonlinear behavior of the section involves geometric as well as material nonlinearity, such as may occur due to section collapse. If only nonlinear material behavior is present, it is simpler to use a shell section integrated during the analysis with the appropriate nonlinear material model.

You must specify a constant section thickness as part of the section definition or a continuously varying thickness by defining the thickness at the nodes as described below. Even though the section’s mechanical behavior is defined in user subroutine UGENS, the thickness of the shell section is required for calculation of the hourglass control stiffness. You must associate this section behavior with a region of your model.

Abaqus/Standard calls user subroutine UGENS for each integration point at each iteration of every increment. The subroutine provides the section state at the start of the increment (section forces and moments, ; generalized section strains, ; solution-dependent state variables; temperature; and any predefined field variables); the increments in temperature and predefined field variables; the generalized section strain increments, ; and the time increment.

The subroutine must perform two functions: it must update the forces, the moments, and the solution-dependent state variables to their values at the end of the increment; and it must provide the section stiffness matrix, . The complete section response, including the thermal expansion effects, must be programmed in the user subroutine.

You should ensure that the strain increment is not used or changed in user subroutine UGENS for linear perturbation analyses. For this case the quantity is undefined.

This method of defining the shell section properties cannot be used with continuum shell elements.

Input File Usage: \*SHELL GENERAL SECTION, ELSET=name, USER

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

Abaqus/CAE Usage: User subroutine UGENS is not supported in Abaqus/CAE.

# Defining whether or not the section stiffness matrices are symmetric

If the section stiffness matrices are not symmetric, you can specify that Abaqus/Standard should use its unsymmetric equation solution capability (see “Defining an analysis,” Section 6.1.2).

Input File Usage: \*SHELL GENERAL SECTION, ELSET=name, USER, UNSYMM

Abaqus/CAE Usage: User subroutine UGENS is not supported in Abaqus/CAE.

<!-- source-page: 459 -->

# Defining the section properties

Any number of constants can be defined to be used in determining the section behavior. You can specify the number of integer property values required, m, and the number of real (floating point) property values required, n; the total number of values required is the sum of these two numbers. The default number of integer property values required is 0, and the default number of real property values required is 0.

Integer property values can be used inside user subroutine UGENS as flags, indices, counters, etc. Examples of real (floating point) property values are material properties, geometric data, and any other information required to calculate the section response in UGENS.

The property values are passed into user subroutine UGENS each time the subroutine is called.

Input File Usage: \*SHELL GENERAL SECTION, ELSET=name, USER, I PROPERTIES=m,PROPERTIES=n

To define the property values, enter all floating point values on the data lines first, followed immediately by the integer values. Eight values can be entered per line.

Abaqus/CAE Usage: User subroutine UGENS is not supported in Abaqus/CAE.

# Defining the number of solution-dependent variables that must be stored for the section

You can define the number of solution-dependent state variables that must be stored at each integration point within the section. There is no restriction on the number of variables associated with a user-defined section. The default number of variables is 1. Examples of such variables are plastic strains, damage variables, failure indices, user-defined output quantities, etc.

These solution-dependent state variables can be calculated and updated in user subroutine UGENS.

Input File Usage: \*SHELL GENERAL SECTION, ELSET=name, USER, VARIABLES=n

Abaqus/CAE Usage: User subroutine UGENS is not supported in Abaqus/CAE.

# Idealizing the section response

Idealizations allow you to modify the stiffness coefficients in a shell section based on assumptions about the shell’s makeup or expected behavior. The following idealizations are available for general shell sections:

• Retain only the membrane stiffness for shells whose predominant response will be in-plane stretching.   
• Retain only the bending stiffness for shells whose predominant response will be pure bending.   
• Ignore the effects of the material layer stacking sequence for composite shells.

The membrane stiffness and bending stiffness idealizations can be applied to homogeneous shell sections, composite shell sections, or shell sections with the stiffness coefficients specified directly. The idealization to ignore stacking effects can be applied only to composite shell sections.

Idealizations modify the shell general stiffness coefficients after they have been computed normally, including the effects of offset.

<!-- source-page: 460 -->

• If you use any idealization, all membrane-bending coupling terms are set to zero.   
• If you retain only the membrane stiffness, off-diagonal terms of the bending submatrix are set to zero, and diagonal bending terms are set to $1 \times 1 0 ^ { - 6 }$ times the largest diagonal membrane coefficient.   
• If you retain only the bending stiffness, off-diagonal terms of the membrane submatrix are set to zero, and diagonal membrane terms are set to $1 \times 1 0 ^ { - 6 }$ times the largest diagonal bending coefficient.   
• If you ignore the material layer stacking sequence in a composite shell, each term of the bending submatrix is set equal to $\scriptstyle { T ^ { 2 } } / 1 2$ times the corresponding membrane submatrix term, where T is the total thickness of the shell.

<table><tr><td>Input File Usage:</td><td>Use the following option to retain only the membrane stiffness:*SHELL GENERAL SECTION, MEMBRANE ONLYUse the following option to retain only the bending stiffness:*SHELL GENERAL SECTION, BENDING ONLYUse the following option to ignore the effects of the layer stacking sequence:*SHELL GENERAL SECTION, COMPOSITE, SMEAR ALL LAYERSMultiple idealization options can be used on the same general shell section.</td></tr><tr><td>Abaqus/CAE Usage:</td><td>Use any of the following options to apply an idealization to a shell section:Property module: Homogeneous shell section editor: Section integration: Before analysis; Basic: Idealization: Membrane only or Bending onlyProperty module: Composite shell section editor: Section integration: Before analysis; Basic: Idealization: Membrane only, Bending only, or Smear all layersProperty module: Shell (conventional or continuum) composite layup editor: Section integration: Before analysis; Basic: Idealization: Membrane only, Bending only, or Smear all layersYou cannot apply multiple idealizations to the same shell section in Abaqus/CAE, and you cannot apply idealizations to a general shell stiffness section.</td></tr></table>

# Defining a shell offset value for conventional shells

You can define the distance (measured as a fraction of the shell’s thickness) from the shell’s midsurface to the reference surface containing the element’s nodes (see “Defining the initial geometry of conventional shell elements,” Section 29.6.3). Positive values of the offset are in the positive normal direction (see “Shell elements: overview,” Section 29.6.1). When the offset is set equal to 0.5, the top surface of the shell is the reference surface. When the offset is set equal to −0.5, the bottom surface is the reference surface. The default offset is 0, which indicates that the middle surface of the shell is the reference surface.
