<!-- source-page: 441 -->

In Gauss quadrature there are no section points on the shell surfaces; therefore, Gauss quadrature should be used only in cases where results on the shell surfaces are not required.

Gauss quadrature cannot be used for heat transfer and coupled temperature-displacement shell elements.

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

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

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

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

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

# 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.

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 29.6.5–2.

Input File Usage: Use the following option to specify a value for the shell offset:

\*SHELL 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.

<!-- source-page: 442 -->

![](images/page-442_eb50c5e5e2291ec0f1a48161659f61718ff279451a31a5a021b617c9997a116e.jpg)

<details>
<summary>text_image</summary>

SPOS
SNEG
SPOS
SNEG
n
n
SPOS
SNEG
n
Mid surface
</details>

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 29.6.5–2 Schematic of shell offset for an offset value of 0.5.

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

Property module: composite layup editor: Section integration:

During 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

<!-- source-page: 443 -->

<table><tr><td>Abaqus/CAE Usage:</td><td>Use the following option for a conventional shell composite layup:Property module: composite layup editor: Section integration: During analysis; Shell Parameters: Shell thickness: Element distribution: select an analytical field or an element-based discrete fieldUse the following option for a homogeneous shell section:Property module: shell section editor: Section integration: During analysis; Basic: Shell thickness: Element distribution: select an analytical field or an element-based discrete fieldUse the following option for a composite shell section:Property module: shell section editor: Section integration: During analysis; Advanced: Shell thickness: Element distribution: select an analytical field or an element-based discrete field</td></tr></table>

# 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. The thickness of continuum shell elements is defined by the element geometry.

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 SECTION, NODAL THICKNESS

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

Property module: composite layup editor: Section integration:

During 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:

During analysis; Basic: Nodal distribution: select an analytical field or a node-based discrete field

<!-- source-page: 444 -->

Use the following option for a composite shell section:

Property module: shell section editor: Section integration: During 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 can be based on a fixed section Poisson’s ratio, either user specified or computed by Abaqus based on the elastic portion of the material definition. Alternatively, in Abaqus/Explicit the Poisson strain can be integrated through the section based on the material response at the individual material points in the section.

By default, Abaqus/Standard computes the Poisson’s strain using a fixed section Poisson’s ratio of 0.5; Abaqus/Explicit uses the material response to compute the Poisson’s strain. See “Finite-strain shell element formulation,” Section 3.6.5 of the Abaqus Theory Guide, for details regarding the underlying formulation.

Input File Usage: Use the following option to specify a value for the effective Poisson’s ratio:

\*SHELL SECTION, POISSON=

Use the following option to cause the shell thickness to change based on the element initial elastic material definition:

\*SHELL SECTION, POISSON=ELASTIC

Use the following option (available only in Abaqus/Explicit) to cause the thickness direction strain under plane stress conditions to be a function of the membrane strains and the in-plane material properties:

\*SHELL SECTION, POISSON=MATERIAL

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

Property module: composite layup editor: Section integration: During 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: During 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.

<!-- source-page: 445 -->

# 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 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: During 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: During analysis; Advanced: Thickness modulus $E _ { e f f }$ to specify the thickness properties directly

You cannot specify a shell thickness direction behavior based on the initial elastic material definition in Abaqus/CAE.

# Defining the transverse shear stiffness

You can provide nondefault values of the transverse shear stiffness. You must specify the transverse shear stiffness in Abaqus/Standard if the section is used with shear flexible shells and the material definitions used in the shell section do not include linear elasticity (“Linear elastic behavior,” Section 22.2.1). See “Shell section behavior,” Section 29.6.4, for more information about transverse shear stiffness.

If you do not specify the transverse shear stiffness values, Abaqus will integrate through the section to determine them. The transverse shear stiffness is precalculated based on the initial elastic material properties, as defined by the initial temperature and predefined field variables evaluated at the midpoint of each material layer. This stiffness is not recalculated during the analysis.

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 the fabric material model or by user subroutine UMAT, UHYPEL, UHYPER, or VUMAT. You must define the transverse shear stiffnesses in such cases except for STRI3 elements.

<!-- source-page: 446 -->

Input File Usage: Use both of the following options: \*SHELL SECTION \*TRANSVERSE SHEAR STIFFNESS

Abaqus/CAE Usage: Use the following option for a composite layup: Property module: composite layup editor: Section integration: During 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: During analysis; Advanced: toggle on Specify transverse shear

# 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 SECTION, CONTROLS=name

Abaqus/CAE Usage: Mesh module: Mesh→Element Type: Element Controls

# Defining density for conventional shells

You can define additional mass per unit area for conventional shell elements directly in the section 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 SECTION, ELSET=name, DENSITY=

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

Property module: composite layup editor: Section integration: During 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: During analysis; Advanced: toggle on Density, and enter

# 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. When the enhanced hourglass control formulation is used with composite

<!-- source-page: 447 -->

shells, the average value of the bulk material properties and the minimum value of the shear material properties over all the layers are used for computing the hourglass forces and moments.

In Abaqus/Standard you can modify the default values for hourglass control stiffness based on the default total stiffness approach for elements that use reduced integration 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.

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. Continuum shell elements do not use a drill stiffness; hence, the scale factor is ignored.

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 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 SECTION

\*HOURGLASS STIFFNESS

# Abaqus/CAE Usage:

Mesh module: Mesh→Element Type: Element Controls

# Specifying temperature and field variables

You can specify temperatures and field variables for conventional shell elements by defining the value at the reference surface of the shell and the gradient through the shell thickness or by defining the values at equally spaced points through each layer of the shell’s thickness. You can specify a temperature gradient only for elements without temperature degrees of freedom. The temperatures and field variables for continuum shell elements are defined at the nodes and then interpolated to the section points.

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).

If temperature is to be read as a predefined field from the results file or the output database file of a previous analysis, the temperature must be defined at equally spaced points through each layer of the

<!-- source-page: 448 -->

thickness. In addition, the results file must be modified so that the field variable data are stored in record 201. See “Predefined fields,” Section 34.6.1, for additional details.

# Defining the value at the reference surface and the gradient through the thickness

You can define the temperature or predefined field by its magnitude on the reference surface of the shell and the gradient through the thickness. If only one value is given, the magnitude will be constant through the thickness.

Input File Usage: Use the following option to specify that the temperatures or predefined fields are defined by a gradient:

\*SHELL SECTION

Use any of the following options to specify the actual values of the temperatures or predefined fields:

\*TEMPERATURE

\*FIELD

\*INITIAL CONDITIONS, TYPE=TEMPERATURE

\*INITIAL CONDITIONS, TYPE=FIELD

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

Property module: composite layup editor: Section integration: During analysis; Shell Parameters; Temperature variation: Linear through thickness

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

Property module: shell section editor: Section integration: During analysis: Advanced; Temperature variation: Linear through thickness

Only initial temperatures and predefined temperature fields are supported in Abaqus/CAE.

Load module: Create Predefined Field: Step: initial\_step or analysis\_step: choose Other for the Category and Temperature for the Types for Selected Step

# Defining the values at equally spaced points through the thickness

Alternatively, you can define the temperature and field variable values at equally spaced points through the thickness of a shell or of each layer of a composite shell.

For a sequentially coupled thermal-stress analysis in Abaqus/Standard, the number (n) of equally spaced points through the thickness of a layer is an odd number when temperature values are obtained from the results file or the output database file generated by a previous Abaqus/Standard heat transfer analysis (since only Simpson’s rule can be used for integration through the section in heat transfer analysis). n may be even or odd if the values are supplied from some other source. In either case Abaqus/Standard interpolates linearly between the two closest defined temperature points to find the temperature values at the section points.

<!-- source-page: 449 -->

The number of predefined field points through each layer, n, must be the same as the number of integration points used through the same layer in the analysis from which the temperatures are obtained. This requirement implies that in the previous analysis each of the layers must have the same number of integration points.

You specify $1 + n _ { l } ( n _ { T } - 1 )$ temperature or field variable values, where $n _ { l }$ is the number of layers in the shell section and $n _ { T } \left( n _ { T } > 1 \right)$ is the value of n. For $n _ { T } { = } 1$ , you specify $n _ { l }$ one temperature or field variable value for a given node or node set.

Input File Usage: Use the following option to specify that the temperatures or predefined fields are defined at equally spaced points:

\*SHELL SECTION, TEMPERATURE=n

Use any of the following options to specify the actual values of the temperatures or predefined fields:

\*TEMPERATURE

\*FIELD

\*INITIAL CONDITIONS, TYPE=TEMPERATURE

\*INITIAL CONDITIONS, TYPE=FIELD

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

Property module: composite layup editor: Section integration: During analysis; Shell Parameters; Temperature variation: Piecewise linear over n values

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

Property module: shell section editor: Section integration: During analysis: Advanced; Temperature variation: Piecewise linear over n values

Only initial temperatures and predefined temperature fields are supported in Abaqus/CAE.

Load module: Create Predefined Field: Step: initial\_step or analysis\_step: choose Other for the Category and Temperature for the Types for Selected Step

# Example

An example of this scheme is illustrated in Figure 29.6.5–3 and Figure 29.6.5–4. The following Abaqus/Standard heat transfer shell section definition corresponds to this example:

\*SHELL SECTION, COMPOSITE

, 3, MAT1, ORI1

, 3, MAT2, ORI2

, 3, MAT3, ORI3

<!-- source-page: 450 -->

![](images/page-450_eb673784ba743ca8d0abe73dfb628d4b6593c5f125808e49fb2536090fc3b5b3.jpg)

<details>
<summary>text_image</summary>

Composite shell section
n
layer 3
t₃
layer 2
t₂
layer 1
Use default of 3 section
points per layer
Specify 3 temperature points
per layer, shared at layer intersections,
7 total
nₜ = 3
nᵢ = 3
1 + nᵢ (nₜ - 1) = 7
</details>

Figure 29.6.5–3 Defining temperature values at n equally spaced points using Simpson’s rule.

This creates degrees of freedom 11–17 in the heat transfer analysis. Temperatures corresponding to these degrees of freedom are then read into the stress analysis at the temperature points shown and interpolated to the section points shown.

# Defining a continuous temperature field

In Abaqus/Standard if an element with temperature degrees of freedom other than a shell abuts the bottom surface of a shell element with temperature degrees of freedom, the temperature field is made continuous when the elements share nodes. If another element with temperature degrees of freedom abuts the top surface, separate nodes must be used and a linear constraint equation (“Linear constraint equations,” Section 35.2.1) must be used to constrain the temperatures to be the same (that is, to give the same value to the top surface degree of freedom on the shell and degree of freedom 11 on the other element).

For the same reason you must be careful if a different number of temperature points is used in adjacent shell elements. For compatibility MPCs (“General multi-point constraints,” Section 35.2.2) or equation constraints are also needed in this case.
