<!-- source-page: 401 -->

<table><tr><td>Load ID (*DLOAD)</td><td>Units</td><td>Description</td></tr><tr><td>CENTRIF</td><td> $T^{-2}$ </td><td>Centrifugal load (magnitude is input as  $\omega^{2}$ , where  $\omega$  is the angular velocity).</td></tr><tr><td>GRAV</td><td> $LT^{-2}$ </td><td>Gravity loading in a specified direction (magnitude is input as acceleration).</td></tr><tr><td>HPE</td><td> $FL^{-2}$ </td><td>Hydrostatic external pressure, with linear variation in global  $Z$  (closed-end condition).</td></tr><tr><td>HPI</td><td> $FL^{-2}$ </td><td>Hydrostatic internal pressure, with linear variation in global  $Z$  (closed-end condition).</td></tr><tr><td>PE</td><td> $FL^{-2}$ </td><td>Uniform external pressure (closed-end condition).</td></tr><tr><td>PI</td><td> $FL^{-2}$ </td><td>Uniform internal pressure (closed-end condition).</td></tr><tr><td>PENU</td><td> $FL^{-2}$ </td><td>Nonuniform external pressure with magnitude supplied via user subroutine DLOAD (closed-end condition).</td></tr><tr><td>PINU</td><td> $FL^{-2}$ </td><td>Nonuniform internal pressure with magnitude supplied via user subroutine DLOAD (closed-end condition).</td></tr><tr><td>ROTA</td><td> $T^{-2}$ </td><td>Rotary acceleration load (magnitude is input as  $\alpha$ , where  $\alpha$  is the rotary acceleration).</td></tr></table>

# Abaqus/Aqua loads

Abaqus/Aqua loads are specified as described in “Abaqus/Aqua analysis,” Section 6.11.1.

<table><tr><td>Load ID(*CLOAD/*DLOAD)</td><td>Units</td><td>Description</td></tr><tr><td> $FDD^{(A)}$ </td><td> $FL^{-1}$ </td><td>Transverse fluid drag load.</td></tr><tr><td> $FD1^{(A)}$ </td><td>F</td><td>Fluid drag force on the first end of the elbow (node 1).</td></tr><tr><td> $FD2^{(A)}$ </td><td>F</td><td>Fluid drag force on the second end of the elbow (node 2 or node 3).</td></tr><tr><td> $FDT^{(A)}$ </td><td> $FL^{-1}$ </td><td>Tangential fluid drag load.</td></tr><tr><td> $FI^{(A)}$ </td><td> $FL^{-1}$ </td><td>Transverse fluid inertia load.</td></tr></table>

<!-- source-page: 402 -->

<table><tr><td>Load ID(*CLOAD/*DLOAD)</td><td>Units</td><td>Description</td></tr><tr><td>FI1(A)</td><td>F</td><td>Fluid inertia force on the first end of the elbow (node 1).</td></tr><tr><td>FI2(A)</td><td>F</td><td>Fluid inertia force on the second end of the elbow (node 2 or node 3).</td></tr><tr><td>PB(A)</td><td>FL-1</td><td>Buoyancy force (closed-end condition).</td></tr><tr><td>WDD(A)</td><td>FL-1</td><td>Transverse wind drag load.</td></tr><tr><td>WD1(A)</td><td>F</td><td>Wind drag force on the first end of the elbow (node 1).</td></tr><tr><td>WD2(A)</td><td>F</td><td>Wind drag force on the second end of the elbow (node 2 or node 3).</td></tr></table>

# Element output

The default stress output points are on the inside surface and the outside surface at all integration stations around the pipe.

# Stress, strain, and other tensor components

Stress and other tensors (including strain tensors) are available for elements with displacement degrees of freedom. All tensors have the same components. For example, the stress components are as follows:

<table><tr><td>S11</td><td>Direct stress along the pipe.</td></tr><tr><td>S22</td><td>Direct stress around the pipe section.</td></tr><tr><td>S12</td><td>Shear stress in the pipe wall.</td></tr></table>

# Section forces and moments

<table><tr><td>SF1</td><td>Axial force.</td></tr><tr><td>SM1</td><td>Bending moment about the local 1-axis.</td></tr><tr><td>SM2</td><td>Bending moment about the local 2-axis.</td></tr><tr><td>SM3</td><td>Twisting moment about the elbow axis.</td></tr></table>

<!-- source-page: 403 -->

# Node ordering on elements

![](images/page-403_3a45052aa5d6992440524b4fac0ec80d33bf45b511940d7aa4d0d60314a0ef58.jpg)

<details>
<summary>natural_image</summary>

Simple diagonal line with two labeled points (1 and 2) on a white background (no text or symbols beyond labels)
</details>

2-node element

![](images/page-403_3dcc83e6f577ed40b8e7e9561cd568b4978e847ec3af66587ee9a39e7d1a8f61.jpg)

<details>
<summary>text_image</summary>

1
2
3
</details>

3-node element

# Numbering of integration points for output

![](images/page-403_6c866e8e5e3deb2ea897ba7db01dd87a711a182c8c2deeccb5acbd7f8e07efdd.jpg)

<details>
<summary>radar</summary>

| Point | Value |
|-------|-------|
| 1     | 1     |
| 2     | 2     |
| 3     | 3     |
| 4     | 4     |
| 5     | 5     |
| 6     | 6     |
| 7     | 7     |
| 8     | 8     |
| 9     | 9     |
| 10    | 10    |
| 11    | 11    |
| 12    | 12    |
| 13    | 13    |
| 14    | 14    |
| 15    | 15    |
| 16    | 16    |
| 17    | 17    |
| 18    | 18    |
| 19    | 19    |
| 20    | 20    |
</details>

![](images/page-403_48b46b52452030c8665c1a7360572fb411c1828bc04b0584f8be4c5f88d2e478.jpg)

<details>
<summary>text_image</summary>

inside
1
outside
5
</details>

The extrados is the side of the pipebend that is furthest away from the center of the torus defining the pipebend; that is, the side of the pipebend to which the $\mathbf { a } _ { 2 }$ -axis points. The intrados is the side of the pipebend closest to the center of the torus.

The middle surface integration points around a section are shown above. There is a default of five thickness direction integration points at each such point, with point 1 on the inside surface of the pipe and point 5 on the outside surface.

<!-- source-page: 404 -->

For ELBOW31 and ELBOW31B only one integration station is used along the axis of the element. For ELBOW32 two integration stations are used along the axis of the elbow and the point numbers on the second section are a continuation of those on the first section (e.g., 21, 22, …, 40 in the default case), located around the pipe as shown above.

<!-- source-page: 405 -->

# 29.6 Shell elements

• “Shell elements: overview,” Section 29.6.1   
• “Choosing a shell element,” Section 29.6.2   
• “Defining the initial geometry of conventional shell elements,” Section 29.6.3   
• “Shell section behavior,” Section 29.6.4   
• “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   
• “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

<!-- source-page: 406 -->

<!-- source-page: 407 -->

# 29.6.1 SHELL ELEMENTS: OVERVIEW

Abaqus offers a wide variety of shell modeling options.

# Overview

Shell modeling consists of:

• choosing the appropriate shell element type (“Choosing a shell element,” Section 29.6.2);   
• defining the initial geometry of the surface (“Defining the initial geometry of conventional shell elements,” Section 29.6.3);   
• determining whether or not numerical integration is needed to define the shell section behavior (“Shell section behavior,” Section 29.6.4); and   
• defining the shell section behavior (“Using a shell section integrated during the analysis to define the section behavior,” Section 29.6.5, or “Using a general shell section to define the section behavior,” Section 29.6.6).

# Conventional shell versus continuum shell

Shell elements are used to model structures in which one dimension, the thickness, is significantly smaller than the other dimensions. Conventional shell elements use this condition to discretize a body by defining the geometry at a reference surface. In this case the thickness is defined through the section property definition. Conventional shell elements have displacement and rotational degrees of freedom.

In contrast, continuum shell elements discretize an entire three-dimensional body. The thickness is determined from the element nodal geometry. Continuum shell elements have only displacement degrees of freedom. From a modeling point of view continuum shell elements look like three-dimensional continuum solids, but their kinematic and constitutive behavior is similar to conventional shell elements.

Figure 29.6.1–1 illustrates the differences between a conventional shell and a continuum shell element.

# Conventions

The conventions that are used for shell elements are defined below.

# Definition of local directions on the surface of a shell in space

The default local directions used on the surface of a shell for definition of anisotropic material properties and for reporting stress and strain components are defined in “Conventions,” Section 1.2.2. You can define other directions by defining a local orientation (see “Orientations,” Section 2.2.5), except for SAX1, SAX2, and SAX2T elements (“Axisymmetric shell element library,” Section 29.6.9), which do not support orientations. A spatially varying local coordinate system defined with a distribution (“Distribution definition,” Section 2.8.1) can be assigned to shell elements. For SAXA elements

<!-- source-page: 408 -->

![](images/page-408_e67fccdfe735c3091b2c0ede3fa0b2941b122d71c104a1b0adf1732e33454f0a.jpg)

<details>
<summary>flowchart</summary>

```mermaid
graph TD
    A["structural body being modeled"] --> B["Conventional shell model - geometry is specified at the reference surface; thickness is defined by section property."]
    A --> C["Finite Element Model"]
    A --> D["Element"]
    B --> E["displacement and rotation degrees of freedom"]
    C --> F["displacement degrees of freedom only"]
    D --> G["continuum shell model - full 3D geometry is specified; element thickness is defined by nodal geometry."]
```
</details>

Figure 29.6.1–1 Conventional versus continuum shell element.

(“Axisymmetric shell elements with nonlinear, asymmetric deformation,” Section 29.6.10) any anisotropic material definition must be symmetric with respect to the r–z plane at and .

In large-deformation (geometrically nonlinear) analysis these local directions rotate with the average rotation of the surface at that point. They are output as directions in the current configuration except in the shell elements in Abaqus/Standard that provide only large rotation but small strain (element types STRI3, STRI65, S4R5, S8R, S8RT, S8R5, S9R5—see “Choosing a shell element,” Section 29.6.2), where they are output as directions in the reference configuration. Therefore, in geometrically nonlinear analysis, when displaying these directions or when displaying principal values of stress, strain, or section forces or moments in Abaqus/CAE, the current (deformed) configuration should be used except for the small-strain elements in Abaqus/Standard, for which the reference configuration should be used.

# Positive normal definition for conventional shell elements

The “top” surface of a conventional shell element is the surface in the positive normal direction and is referred to as the positive (SPOS) face for contact definition. The “bottom” surface is in the negative direction along the normal and is referred to as the negative (SNEG) face for contact definition. Positive and negative are also used to designate top and bottom surfaces when specifying offsets of the reference surface from the shell’s midsurface.

The positive normal direction defines the convention for pressure load application and output of quantities that vary through the thickness of the shell. A positive pressure load applied to a shell element produces a load that acts in the direction of the positive normal.

<!-- source-page: 409 -->

# Three-dimensional conventional shells

For shells in space the positive normal is given by the right-hand rule going around the nodes of the element in the order that they are specified in the element definition. See Figure 29.6.1–2.

![](images/page-409_64e852481574c64b5d04d5d585142c81a01430fccb06c5e6deb803aa6850cf93.jpg)

<details>
<summary>text_image</summary>

face SPOS
face SNEG
</details>

Figure 29.6.1–2 Positive normals for three-dimensional conventional shells.

# Axisymmetric conventional shells

For axisymmetric conventional shells (including the SAXA1n and SAXA2n elements that allow for nonsymmetric deformation) the positive normal direction is defined by a 90° counterclockwise rotation from the direction going from node 1 to node 2. See Figure 29.6.1–3.

![](images/page-409_8bab9494a923ac583335b6c5611e74e39cfadff5d7651e0ed4783c346f92178d.jpg)

<details>
<summary>text_image</summary>

face SPOS
2
face SNEG
1
z
r
n
</details>

Figure 29.6.1–3 Positive normal for conventional axisymmetric shells.

# Normal definition for continuum shell elements

Figure 29.6.1–4 illustrates the key geometrical features of continuum shells. It is important that the continuum shells are oriented properly, since the behavior in the thickness direction is different from that in the in-plane directions. By default, the element top and bottom faces and, hence, the element normal, stacking direction, and thickness direction are defined by the nodal connectivity. For the triangular inplane continuum shell element (SC6R) the face with corner nodes 1, 2, and 3 is the bottom face; and the face with corner nodes 4, 5, and 6 is the top face. For the quadrilateral continuum shell element (SC8R)

<!-- source-page: 410 -->

![](images/page-410_600d09387e94d9a4bf98d7b4a5c736db4c4c725ad131adff1c5ab16241a78363.jpg)

<details>
<summary>text_image</summary>

thickness
direction
5
1
8
n
4
7
top face
2
3
4
1
6
3
bottom face
5
2
thickness
direction
z
y
x
</details>

Figure 29.6.1–4 Default normals and thickness direction for continuum shell elements.

the face with corner nodes 1, 2, 3, and 4 is the bottom face; and the face with corner nodes 5, 6, 7, and 8 is the top face. The stacking direction and thickness direction are both defined to be the direction from the bottom face to the top face. Additional options for defining the element thickness direction, including one option that is independent of nodal connectivity, are presented below.

Surfaces on continuum shells can be defined by specifying the face identifiers S1–S6 identifying the individual faces as defined in “Continuum shell element library,” Section 29.6.8. Free surface generation can also be used.

Pressure loads applied to faces P1–P6 are defined similar to continuum elements, with a positive pressure directed into the element.

# Defining the stacking and thickness direction

By default, the continuum shell stacking direction and thickness direction are defined by the nodal connectivity as illustrated in Figure 29.6.1–4. Alternatively, you can define the element stacking direction and thickness direction by either selecting one of the element’s isoparametric directions or by using an orientation definition.

# Defining the stacking and thickness direction based on the element isoparametric direction

You can define the element stacking direction to be along one of the element’s isoparametric directions (see Figure 29.6.1–5 for element stack directions). The 8-node hexahedron continuum shell has three possible stacking directions; the 6-node in-plane triangular continuum shell has only one stack direction, which is in the element 3-isoparametric direction. The default stacking direction is 3, providing the same thickness and stacking direction as outlined in the previous section.

To obtain a desired thickness direction, the choice of the isoparametric direction depends on the element connectivity. For a mesh-independent specification, use an orientation-based method as described below.

# Input File Usage:

Use one of the following options to define the element stacking direction based on the element’s isoparametric directions:
