SHELL209 Element Description

The SHELL209 element is suitable for analyzing thin to moderately thick axisymmetric shell structures. It is a three-node element with three degrees of freedom at each node: translations in the X, Y directions, and a 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. (For higher efficiency, the two-node element SHELL208 may be more suitable.)

The element is well suited for linear, large rotation, and/or large strain nonlinear applications. Changes in shell thickness and follower effects of distributed pressures are accounted for in nonlinear analyses, and it can be used for layered applications for modeling laminated composite shells or sandwich construction. See SHELL209 for more details about this element.

Figure 209.1: SHELL209 Geometry

SHELL209 Input Data

Figure 209.1: SHELL209 Geometry shows the geometry, node locations, and element coordinate system for this element. The element is defined by three 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 Element Loading. Pressure may be input as surface loads on the element faces as shown by the circled numbers on Figure 209.1: SHELL209 Geometry. Positive pressures act into the element.

Temperatures can 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, T2, and T3; T2 (as input) is used for T4, T5, and T6, 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).

To evaluate stresses and strains on exterior surfaces, set KEYOPT(1) = 2. When used as overlaid elements on the faces of 2D axisymmetric elements, this option is similar to the surface stress option, but is more general and applicable to nonlinear analysis. The element used with this option provides no stiffness, mass, or load contributions. Use this option in single-layer shells only. Irrespective of other settings, SHELL208 provides stress and strain output at the center of the layer.

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.

SHELL209 includes the effects of transverse shear deformation. The transverse shear stiffness E11 can be specified with 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.

SHELL209 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 INISTATE. For more information, see Initial State in the 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.

The element supports both consistent and lumped mass matrices. Issue LUMPM,ON to activate a lumped mass matrix. A consistent mass matrix is used by default.

"SHELL209 Input Summary" gives a summary of the element input. A general description of element input is given in Element Input

SHELL209 Output Data

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

Several items are illustrated in Figure 209.2: SHELL209 Element Stress Output.

KEYOPT(8) controls the amount of data output on the result file for processing with LAYER. 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 are 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).

Mechanical APDL calculates moments (M11, M22) with respect to the shell reference plane. By default, the program adopts the shell midplane as the reference plane. To offset the reference plane to any other specified location, issue SECOFFSET. 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:

SHELL209 does not support extensive basic element printout. POST1 provides more comprehensive output processing tools; therefore, consider issuing OUTRES to ensure that the required results are stored in the database.

Figure 209.2: SHELL209 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 letter or number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 209.2: SHELL209 Item and Sequence Numbers lists output available via ETABLE 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 209.2: SHELL209 Item and Sequence Numbers:

SHELL209 Assumptions and Restrictions

SHELL209 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  —