SHELL208

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 in the *Mechanical APDL Theory Reference* for more details about this element.

Figure 208.1 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 **SECCONTROLS**). 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. 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). 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 **SECCONTROLS**. 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.

You can apply an initial stress state to this element via the **INISTATE** command. For more information, see "Initial State" in the *Basic 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.

**Nodes**I, J

**Degrees of Freedom**UX, UY, ROTZ -- If KEYOPT(1) = 0 and KEYOPT(2) = 0 UX, UY -- If KEYOPT(1) = 1 and KEYOPT(2) = 0 UX, UY, UZ, ROTZ -- If KEYOPT(1) = 0 and KEYOPT(2) = 1 UX, UY, UZ -- If KEYOPT(1) = 1 and KEYOPT(2) = 1 **Real Constants**None

**Section Controls**E11, ADMSUA

**Material Properties**EX, EY, EZ, PRXY, PRYZ, PRXZ (or NUXY, NUYZ, NUXZ), ALPX, ALPY, ALPZ (or CTEX, CTEY, CTEZ or THSX, THSY, THSZ), DENS, GXY, GYZ, GXZ, ALPD, BETD **Surface Loads****Pressures --**face 1 (I-J) (top, in -N direction), face 2 (I-J) (bottom, in +N direction)

**Body Loads****Temperatures --**For KEYOPT(1) = 0: T1, T2 (corresponding to nodes I and J) at bottom of layer 1, and T3, T4 (corresponding to nodes I and J) between layers 1-2. A similar relationship exists for all layers, ending with temperatures at the top of layer NL. Hence, for one-layer elements, four temperatures are used. For KEYOPT(1) = 1: T1, T2 for layer 1; T3, T4 for layer 2; similarly for all layers (2 * NL maximum). Hence, for one-layer elements, two temperatures are used.

**Special Features****KEYOPT(1)**Element stiffness:

**0 --**Bending and membrane stiffness (default).

**1 --**Membrane stiffness only.

**KEYOPT(2)**Torsion capability:

**0 --**Excluded (default).

**1 --**Included.

**KEYOPT(3)**Extra internal node option:

**0 --**Suppress extra internal node (default).

**2 --**Include extra internal node.

**KEYOPT(8)**Storage of layer data:

**0 --**Store data for BOTTOM of bottom layer and TOP of top layer (default).

**1 --**Store data for TOP and BOTTOM for all layers.

**2 --**Store data for TOP, BOTTOM, and MID for all layers. (The volume of data may be excessive.)

**KEYOPT(9)**User-defined thickness:

**0 --**No user subroutine to provide initial thickness (default).

**1 --**Read initial thickness data from user subroutine UTHICK

See the

*Guide to ANSYS User Programmable Features*for information about user-written subroutines

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

Nodal displacements included in the overall nodal solution.

Additional element output as shown in Table 208.1: SHELL208 Element Output Definitions

Several items are illustrated in Figure 208.2.

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 γ_{13} 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.

**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 208.1 SHELL208 Element Output Definitions**

Name | Definition | O | R |
---|---|---|---|

EL | Element Number | Y | Y |

NODES | Nodes - I, J | - | Y |

MAT | Material number | - | Y |

THICK | Average thickness | - | Y |

VOLU: | Volume | - | Y |

XC, YC | Location where results are reported | Y | 4 |

PRES | Pressures P1 (top) at NODES I, J; P2 (bottom) at NODES I, J | - | Y |

TEMP | Temperatures T1, T2 at bottom of layer 1, T3, T4 between layers 1-2, similarly for between next layers, ending with temperatures at top of layer NL (2*(NL+1) maximum) | - | Y |

LOC | TOP, MID, BOT, or integration point location | - | 1 |

S:X, Y, Z, XY, YZ, XZ | Stresses | 3 | 1 |

S:1, 2, 3 | Principal stresses | - | 1 |

S:INT | Stress intensity | - | 1 |

S:EQV | Equivalent stress | - | 1 |

EPEL:X, Y, Z, XY,YZ,XZ | Elastic strains | 3 | 1 |

EPEL:EQV | Equivalent elastic strain | - | 1 |

EPTH:X, Y, Z, XY,YZ,XZ | Thermal strains | 3 | 1 |

EPTH:EQV | Equivalent thermal strain | - | 1 |

EPPL:X, Y, Z, XY,YZ,XZ | Average plastic strains | 3 | 2 |

EPPL:EQV | Equivalent plastic strain | - | 2 |

EPCR:X, Y, Z, XY ,YZ,XZ | Average creep strains | 3 | 2 |

EPCR:EQV | Equivalent creep strain | - | 2 |

EPTO:X, Y, Z ,XY,YZ,XZ | Total mechanical strains (EPEL+EPPL+EPCR) | 3 | - |

EPTO:EQV | Total equivalent mechanical strains | - | - |

NL:EPEQ | Accumulated equivalent plastic strain | - | 2 |

NL:CREQ | Accumulated equivalent creep strain | - | 2 |

NL:SRAT | Plastic yielding (1 = actively yielding, 0 = not yielding) | - | 2 |

NL:PLWK | Plastic work | - | 2 |

NL:HPRES | Hydrostatic pressure | - | 2 |

SEND:Elastic, Plastic, Creep | Strain energy densities | - | 2 |

N11, N22, N12 | In-plane forces (per unit length) | - | Y |

M11, M22 | Out-of-plane moments (per unit length) | - | Y |

Q13 | Transverse shear forces (per unit length) | - | Y |

E11, E22, E12 | Membrane strains | - | Y |

K11, K22 | Curvatures | - | Y |

γ_{13} | Transverse shear strain | - | Y |

LOCI:X, Y, Z | Integration point locations | - | 5 |

SVAR:1, 2, ... , N | State variables | - | 6 |

ILSXZ | SXZ interlaminar shear stress | - | Y |

ILSYZ | SYZ interlaminar shear stress | - | Y |

ILSUM | Magnitude of the interlaminar shear stress vector | - | Y |

ILANG | Angle of interlaminar shear stress vector (measured from the element x-axis toward the element y-axis in degrees) | - | Y |

Sm: 11, 22, 12 | Membrane stresses | - | Y |

Sb: 11, 22 | Bending stresses | - | Y |

Sp: 11, 22, 12 | Peak stresses | - | Y |

St: 13 | Averaged transverse shear stresses | - | Y |

The following stress solution repeats for top, middle, and bottom surfaces.

Nonlinear solution output for top, middle, and bottom surfaces, if the element has a nonlinear material, or if large-deflection effects are enabled (

**NLGEOM**,ON) for SEND.Stresses, total strains, plastic strains, elastic strains, creep strains, and thermal strains in the element coordinate system are available for output (at all section points through thickness). If layers are in use, the results are in the layer coordinate system.

Available only at centroid as a

***GET**item.Available only if

**OUTRES**,LOCI is used.Available only if the UserMat subroutine and

**TB**,STATE command are used.

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) in the *Basic Analysis Guide* and The Item and Sequence Number Table of
this manual for more information. The following notation is used
in Table 208.2: SHELL208 Item and Sequence Numbers:

**Name**output quantity as defined in the Table 208.1: SHELL208 Element Output Definitions

**Item**predetermined Item label for

**ETABLE**command**E**sequence number for single-valued or constant element data

**I, J**sequence number for data at nodes I, J.

**Table 208.2 SHELL208 Item and Sequence Numbers**

Output Quantity Name | ETABLE and ESOL Command Input | |||
---|---|---|---|---|

Item | E | I | J | |

N11 | SMISC | 1 | - | - |

N22 | SMISC | 2 | - | - |

N12 | SMISC | 3 | - | - |

M11 | SMISC | 4 | - | - |

M22 | SMISC | 5 | - | - |

Q13 | SMISC | 6 | - | - |

ε_{11} | SMISC | 7 | - | - |

ε_{22} | SMISC | 8 | - | - |

ε_{12} | SMISC | 9 | - | - |

k_{11} | SMISC | 10 | - | - |

k_{22} | SMISC | 11 | - | - |

γ_{13} | SMISC | 12 | - | - |

THICK | SMISC | 13 | - | - |

P1 | SMISC | - | 14 | 15 |

P2 | SMISC | - | 16 | 17 |

Sm: 11 | SMISC | 18 | - | - |

Sm: 22 | SMISC | 19 | - | - |

Sm: 12 | SMISC | 20 | - | - |

Sb: 11 | SMISC | 21 | - | - |

Sb: 22 | SMISC | 22 | - | - |

Sp: 11 (at shell bottom) | SMISC | 23 | - | - |

Sp: 22 (at shell bottom) | SMISC | 24 | - | - |

Sp: 12 (at shell bottom) | SMISC | 25 | - | - |

Sp: 11 (at shell top) | SMISC | 26 | - | - |

Sp: 22 (at shell top) | SMISC | 27 | - | - |

Sp: 12 (at shell top) | SMISC | 28 | - | - |

St: 13 | SMISC | 29 | - | - |

Output Quantity Name | ETABLE and ESOL Command Input | ||||

Item | Bottom of Layer i | Top of Layer
NL | |||

ILSXZ | SMISC | 8 * (i - 1) + 31 | 8 * (NL - 1) + 32 | ||

ILSYZ | SMISC | 8 * (i - 1) + 33 | 8 * (NL - 1) + 34 | ||

ILSUM | SMISC | 8 * (i - 1) + 35 | 8 * (NL - 1) + 36 | ||

ILANG | SMISC | 8 * (i - 1) + 37 | 8 * (NL - 1) + 38 |

The axisymmetric shell element must be defined in the global X-Y plane with the Y-axis the axis of symmetry.

The element cannot have a zero length.

Zero thickness elements, or elements tapering down to a zero thickness at any corner, are not allowed (but zero thickness layers are allowed).

If multiple load steps are used, the number of layers may not change between load steps.

No slippage is assumed between the element layers. Shear deflections are included in the element; however, normals to the center plane before deformation are assumed to remain straight after deformation.

Transverse shear stiffness of the shell section is estimated by an energy equivalence procedure (of the generalized section forces & strains vs. the material point stresses and strains). The accuracy of this calculation may be adversely affected if the ratio of material stiffnesses (Young's moduli) between adjacent layers is very high.

The calculation of interlaminar shear stresses is based on simplifying assumptions of unidirectional, uncoupled bending in each direction. If accurate edge interlaminar shear stresses are required, shell-to-solid submodeling should be used.

The section definition permits use of hyperelastic material models and elastoplastic material models in laminate definition. However, the accuracy of the solution is primarily governed by fundamental assumptions of shell theory. The applicability of shell theory in such cases is best understood by using a comparable solid model.

For nonlinear applications, this element works best with full Newton-Raphson solution scheme (

**NROPT**,FULL,ON).Stress stiffening is always included in geometrically nonlinear analyses (

**NLGEOM**,ON). Prestress effects can be activated by the**PSTRES**command.In a nonlinear analysis, the solution process terminates if the thickness at any integration point that was defined with a nonzero thickness vanishes (within a small numerical tolerance).

SHELL208 with an internal node cannot be used in substructures.

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 Professional. **

The only special features allowed are stress stiffening and large deflections.