SHELL208 Element Description

The SHELL208 element is suitable for modeling thin to moderately thick axisymmetric shell structures, such as oil tanks, pipes, and cooling towers. It is a two-node element with three degrees of freedom at each node: translations in the x, and y directions, and rotation about the z-axis. A fourth translational degree of freedom in z direction can be included to model uniform torsion (KEYOPT(2) = 1). When the membrane option is used, the rotational degree of freedom is excluded. An extra internal node is available via KEYOPT(3) = 2. (SHELL209 incorporates this extra node by default.)

SHELL208 allows you to account for large strain effects, transverse shear deformation, hyperelasticity and layers in your models. The element is intended to model finite strain with pure axisymmetric displacements; transverse shear strains are assumed to be small.

SHELL208 can be used for layered applications for modeling laminated composite shells or sandwich construction. See SHELL208 for more details about this element.

Figure 208.1:  SHELL208 Geometry

SHELL208 Input Data

Figure 208.1: SHELL208 Geometry shows the geometry, node locations, and element coordinate system for SHELL208. The element is defined by two nodes. For material property labels, the local x-direction corresponds to the meridional direction of the shell element. The local y-direction is the circumferential. The local z-direction corresponds to the through-the-thickness direction. Element formulation is based on logarithmic strain and true stress measures. Element kinematics allows for finite membrane strains (stretching). However, the curvature changes within an increment are assumed to be small.

The shell thickness and more general properties (such as material and number of integration points through the thickness) are specified via section commands (SECTYPE, SECDATA and SECCONTROL). Shell section commands allow for both single-layered and composite shell definitions. You can designate the number of integration points (1, 3, 5, 7, or 9) located through the thickness of each layer. If only one, the integration point is always located midway between the top and the bottom surfaces. If three or more, two points are located on the top and the bottom surfaces respectively and the remaining points are distributed evenly between these two points. The default for each layer is three integration points. The element can have variable thickness, as a tabular function of global/local coordinates or node numbers (SECFUNCTION).

Element loads are described in Nodal Loading. Pressure may be input as surface loads on the element faces as shown by the circled numbers on Figure 208.1: SHELL208 Geometry. Positive pressures act into the element.

Temperatures may be input as element body loads at the corners of the outside faces of the element and the corners of the interfaces between layers. The first corner temperature T1 defaults to TUNIF. If all other temperatures are unspecified, they default to T1. If KEYOPT(1) = 0 and exactly NL+1 (where NL is the number of layers in the shell section) temperatures are input, one temperature is used for the bottom corners of each layer, and the last temperature is for the top corners of the top layer. If KEYOPT(1) = 1 and if exactly NL temperatures are input, one temperature is used for the two corners of each layer; that is, T1 is used for T1 and T2; T2 (as input) is used for T3 and T4, etc. For any other input patterns, unspecified temperatures default to TUNIF.

Nodal forces, if any, should be input on a full 360° basis.

KEYOPT(1) is the membrane option. When KEYOPT(1) = 1, the element uses one integration point through-the-thickness and accounts for only membrane stiffness (that is, the bending and transverse shear stiffness are ignored).

KEYOPT(2) controls the torsion capability. When KEYOPT(2) = 1, the element allows constant torsion by allowing a translational degree of freedom UZ in the circumferential direction.

KEYOPT(3) is used to include or suppress internal nodes. When KEYOPT(3) = 2, the element contains an extra internal node and adopts a two-point integration rule. By default, the element uses one-point integration scheme. (See Figure 208.1: SHELL208 Geometry.) Internal nodes are not accessible to users. Therefore, boundary conditions/loading can not be specified on those nodes.

SHELL208 includes the effects of transverse shear deformation. The transverse shear stiffness E11 can be specified using SECCONTROL. For a single-layered shell with isotropic material, default transverse shear stiffness is kGh, in which k = 5/6, G is the shear modulus, and h is the thickness of the shell.

SHELL208 can be associated with linear elastic, elastoplastic, creep, or hyperelastic material properties.

Set KEYOPT(8) = 2 to store midsurface results in the results file for single- or multi-layer shell elements. If you use SHELL,MID, you will see these calculated values, rather than the average of the TOP and BOTTOM results. You should use this option to access these correct midsurface results (membrane results) for those analyses where averaging TOP and BOTTOM results is inappropriate. Examples include midsurface stresses and strains with nonlinear material behavior, and midsurface results after mode combinations that involve squaring operations such as in spectrum analyses.

Set KEYOPT(9) = 1 to read initial thickness data from a user subroutine.

KEYOPT(10) = 1 outputs normal stress component Sz, where z is shell normal direction. The element uses a plane-stress formulation that always leads to zero thickness normal stress. With KEYOPT(10) = 1, Sz is independently recovered during the element solution output from the applied pressure load.

You can apply an initial stress state to this element via the INISTATE command. For more information, see Initial State in the Mechanical APDL Advanced Analysis Guide.

The effects of pressure load stiffness are automatically included for this element. If an unsymmetric matrix is needed for pressure load stiffness effects, use NROPT,UNSYM.

A summary of the element input is given in "SHELL208 Input Summary". A general description of element input is given in Element Input.

SHELL208 Output Data

The solution output associated with the element is in two forms:

Several items are illustrated in Figure 208.2: SHELL208 Element Stress Output.

KEYOPT(8) controls the amount of data output on the result file for processing with the LAYER command. Interlaminar shear stress is available at the layer interfaces. Setting KEYOPT(8) = 1 or 2 is necessary for these stresses to be output in POST1. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to view results.

The element stress resultants (N11, M11, Q13, etc.) are parallel to the element coordinate system, as are the membrane strains and curvatures of the element. Such generalized strains are available through the SMISC option at the element centroid only. The transverse shear force Q13 is available only in resultant form: that is, use SMISC,5. Likewise, the transverse shear strain γ₁₃ is constant through the thickness and only available as a SMISC item (SMISC,10).

ANSYS computes moments (M11, M22) with respect to the shell reference plane. By default, ANSYS adopts the shell midplane as the reference plane. To offset the reference plane to any other specified location, issue the SECOFFSET command. When there is a nonzero offset (L) from the reference plane to the midplane, moments with respect to the midplane ( ) can be recovered from stress resultants with respect to the reference plane as follows:

SHELL208 does not support extensive basic element printout. POST1 provides more comprehensive output processing tools; you should use the OUTRES command to ensure that the required results are stored in the database.

Figure 208.2:  SHELL208 Element Stress Output

The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates that the item can be accessed by the Component Name method (ETABLE, ESOL). The O column indicates the availability of the items in the file Jobname.OUT. The R column indicates the availability of the items in the results file.

In either the O or R columns, “Y” indicates that the item is always available, a number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 208.2: SHELL208 Item and Sequence Numbers lists output available through the ETABLE command using the Sequence Number method. See The General Postprocessor (POST1) and The Item and Sequence Number Table in this reference for more information. The following notation is used in Table 208.2: SHELL208 Item and Sequence Numbers:

SHELL208 Assumptions and Restrictions

SHELL208 Product Restrictions

When used in the product(s) listed below, the stated product-specific restrictions apply to this element in addition to the general assumptions and restrictions given in the previous section.

ANSYS Mechanical Pro 

ANSYS Mechanical Premium