In this blog we will understand about shell elements. Abaqus offers a wide variety of shell modeling options.

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 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.

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.

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 2.

Normal definition for continuum shell elements

Figure 3 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 in-plane 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) 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.

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 3. 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 4 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.

Choosing a shell element

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.

Naming convention

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:

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.

 “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, S4, S4R, S4RS, S4RSW, SAX1, SAX2, SAX2T, SC6R, and SC8R are general-purpose shells.

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.

Five degree of freedom shells versus six degree of freedom shells

Two types of three-dimensional conventional shell elements are provided in Abaqus/Standard: ones that use five degrees of freedom (three displacement components and two in-surface rotation components) where possible and ones that use six degrees of freedom (three displacement components and three rotation components) at all nodes.

The elements that use five degrees of freedom (S4R5, STRI65, S8R5, S9R5) can be more economical. However, they are available only as “thin” shells (they cannot be used as “thick” shells) and cannot be used for finite-strain applications (although they model large rotations with small strains accurately). In addition, output for the five degree of freedom shell elements is restricted as follows:

• At nodes that use the two in-surface rotation components, the values of these in-surface rotations are not available for output.
• When output variable NFORC is requested, moments corresponding to the in-surface rotations are not available for output.

When five degree of freedom shell elements are used, Abaqus/Standard will automatically switch to using three global rotation components at any node that:

• has kinematic boundary conditions applied to rotational degrees of freedom,
• is used in a multi-point constraint that involves rotational degrees of freedom,
• is shared with a beam element or a shell element that uses the three global rotation components at all nodes,
• is on a fold line in the shell (that is, on a line where shells with different surface normals come together), or
• is loaded with moments.

In all elements that use three global rotation components at all nodes (whether activated as described above or always present), a singularity exists at any node where the surface is assumed to be continuously curved: three rotation components are used, but only two are actively associated with stiffness. A small stiffness is associated with the rotation about the normal to avoid this difficulty. The default stiffness values used are sufficiently small such that the artificial energy content is negligible. In some rare cases this stiffness may need to be altered.

👉 In 3DEXPERIENCE Platform, Mesh visualization orientation can be checked as follows: