Choosing a shell element

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.

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) 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) is degree of freedom 11. The temperature on the top surface is degree of freedom $10+n_s$. 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,

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).

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

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). 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).

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.

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.

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.

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, Finite-strain shell element formulation, and Axisymmetric shell element allowing asymmetric loading.

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.

In Abaqus/Standard the three-dimensional “thick” and “thin” element types STRI3, S4R5, STRI65, S8R, S8RT, S8R5, and S9R5 provide for arbitrarily large rotations but only small strains. The change in thickness with deformation is ignored in these elements.

In Abaqus/Explicit element types S3RS, S4RS, and S4RSW are provided for shell problems with small membrane strains and arbitrarily large rotations. Many impact dynamics analyses fall within this class of problems, including those of shell structures undergoing large-scale buckling behavior but relatively small amounts of membrane stretching and compression. Although solution accuracy may degrade as membrane strains become large, the small-strain shell elements in Abaqus/Explicit provide a computationally efficient alternative to the finite-membrane-strain elements for appropriate applications. The underlying formulation is described in Small-strain shell elements in Abaqus/Explicit.

Thickness change is considered only in geometrically nonlinear analyses. For conventional shells, stress in the thickness direction is zero and the strain results only from the Poisson’s effect. For continuum shells, the stress in the thickness direction may not be zero and may cause additional strain beyond that due to Poisson’s effect. The thickness strain due to Poisson’s effect is referred as the “Poisson strain,” and any additional strain beyond the “Poisson strain” is referred to as the “effective thickness strain.”

For shell elements in Abaqus/Explicit defined by integrating the section during the analysis, the Poisson strain is calculated by enforcing the plane stress condition either at the individual material points in the section and then integrating the Poisson strain from these material points, or at the integration station for the whole section using a “section Poisson’s ratio.” For shell elements in Abaqus/Standard only the section Poisson’s ratio method is available. For shell elements defined by general shell sections, only the section Poisson’s ratio method is applicable.

See Defining the Poisson strain in shell elements in the thickness direction and Defining the Poisson strain in shell elements in the thickness direction for details.

The thickness direction stress is computed by penalizing the effective thickness strain with a constant “thickness modulus.” The thickness modulus used for a single layer shell element with an elastic or elastic-plastic material is twice the in-plane elastic shear modulus. In the case of a composite shell with each layer either an elastic or elastic-plastic material, the thickness modulus is computed as the thickness-weighted harmonic mean of the contributions from the individual layers:

where $E_{eff}$ is the thickness modulus, $i$ is the layer index, $n$ is the number of layers, $r_i$ is the relative thickness of layer $i,(0<r_i<1)$, and $E_{eff}^i$ is twice the initial in-plane elastic shear modulus based on the material definition for layer $i$ in the initial configuration.

See Defining the thickness modulus in continuum shell elements and Defining the thickness modulus in continuum shell elements for details.

Both S3 and S3R refer to the same 3-node triangular shell element. This element is a degenerated version of S4R that is fully compatible with S4R and, in Abaqus/Standard, S4.

Element S3RS, available in Abaqus/Explicit, is a degenerated version of S4RS that is fully compatible with S4RS.

S3/S3R and S3RS provide accurate results in most loading situations. However, because of their constant bending and membrane strain approximations, high mesh refinement may be required to capture pure bending deformations or solutions to problems involving high strain gradients. A consequence of the degenerated element formulation is that the solution changes slightly when the element connectivity is permuted.

Element types S4, S4R, S4R5, S4RS, S8R5, and S9R5 can be degenerated to triangles. However, for elements S4 (element S4 degenerated to a triangle may exhibit overly stiff response in membrane deformation), S4R, and S4RS it is recommended that S3R and S3RS be used instead.

The quarter-point technique (moving the midside nodes to the quarter points to give a $1/\sqrt{r}$ singularity for elastic fracture mechanics applications) can be used with the quadratic element types S8R5 and S9R5 (see Element definition). The accuracy of the element is very significantly reduced when it is degenerated to a triangle; therefore, this is not recommended except for special applications, such as fracture.

Element types S8R and S8RT cannot be degenerated to triangles. Element types DS4 and DS8 can be degenerated to triangles, but it is recommended that DS3 and DS6 elements be used instead.

Continuum shell elements are similar to continuum solids from a modeling point of view. The element geometries for the SC6R and SC8R elements are a triangular prism and hexahedron, respectively, with displacement degrees of freedom only.

Continuum shell elements must be oriented correctly, since these elements have a thickness direction associated with them. See About shell elements for further details on element connectivity and orientation.

When classical shell structures (structures in which only the midsurface geometry and kinematic constraints are provided) are analyzed, care must be taken that appropriate moments and rotations are specified. For example, a moment may be applied as a force-couple system at the corresponding nodes on the top and bottom faces. A rotation boundary condition may be specified through a kinematic constraint to yield the appropriate displacement boundary conditions on the edge of the continuum shell.

Continuum shell elements can be connected directly to first-order continuum solids without any kinematic transition. An appropriate kinematic transition needs to be provided when conventional shell elements are connected to continuum shell elements to correctly transfer the moment/rotation at the reference surface of a conventional shell. Such a transition can be defined with a shell-to-solid coupling constraint or any other kinematic constraint, such as a surface-based coupling constraint, a multi-point constraint, or a linear constraint equation.

For a “sandwich” shell, in which parts of the cross-section are made of a softer material (especially when the layers are nonisotropic so that some layers are weak in particular directions), the transverse shear flexibility can be important even when the shell is rather thin. Use of general-purpose shell elements or stacking continuum shell elements is recommended in such cases. See Shell section behavior for a discussion of transverse shear stiffness in shell elements.

In Abaqus/Standard curved elements (STRI65, S8R5, S9R5) are preferable for modeling bending of a thin curved shell.

Element type STRI3 is a flat facet element. If this element is used to model bending of a curved shell, a dense mesh may be required to obtain accurate results.

Element type S8R5 may give inaccurate results for buckling problems of doubly curved shells due to the fact that the internally defined center node may not be positioned on the actual shell surface. Element type S9R5 should be used instead.

Element type S8R5 is converted automatically to element type S9R5 if a slave surface in a contact pair is attached to the element.

Moments should not be applied to the center node of S9R5 elements.

Element type S4 is a fully integrated, general-purpose, finite-membrane-strain shell element. The element's membrane response is treated with an assumed strain formulation that gives accurate solutions to in-plane bending problems, is not sensitive to element distortion, and avoids parasitic locking.

Element type S4 does not have hourglass modes in either the membrane or bending response of the element; hence, the element does not require hourglass control. The element has four integration locations per element compared with one integration location for S4R, which makes the element computationally more expensive. S4 is compatible with both S4R and S3R. S4 can be used for problems prone to membrane- or bending-mode hourglassing, in areas where greater solution accuracy is required, or for problems where in-plane bending is expected. In all of these situations S4 will outperform element type S4R. S4 cannot be used with the hyperelastic or hyperfoam material definitions in Abaqus/Standard.