SHELL208

2-Node Axisymmetric Shell
MP ME ST PR PRN <> <> <> <> <> <> PP <> EME MFS

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

Figure 208.1  SHELL208 Geometry

SHELL208 Geometry

SHELL208 Input Data

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.

SHELL208 Input Summary

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
Birth and death
Elasticity
Element technology autoselect
Hyperelasticity
Initial state
Large deflection
Large strain
Linear perturbation
Nonlinear stabilization
Plasticity
Stress stiffening
User-defined material
Viscoelasticity
Viscoplasticity / Creep
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

SHELL208 Output Data

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

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 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

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 208.1  SHELL208 Element Output Definitions

NameDefinitionOR
ELElement NumberYY
NODESNodes - I, J-Y
MATMaterial number-Y
THICKAverage thickness-Y
VOLU:Volume-Y
XC, YCLocation where results are reportedY4
PRESPressures P1 (top) at NODES I, J; P2 (bottom) at NODES I, J-Y
TEMPTemperatures 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
LOCTOP, MID, BOT, or integration point location-1
S:X, Y, Z, XY, YZ, XZStresses31
S:1, 2, 3Principal stresses-1
S:INTStress intensity-1
S:EQVEquivalent stress-1
EPEL:X, Y, Z, XY,YZ,XZElastic strains 31
EPEL:EQVEquivalent elastic strain-1
EPTH:X, Y, Z, XY,YZ,XZThermal strains31
EPTH:EQVEquivalent thermal strain-1
EPPL:X, Y, Z, XY,YZ,XZAverage plastic strains32
EPPL:EQV Equivalent plastic strain-2
EPCR:X, Y, Z, XY ,YZ,XZAverage creep strains32
EPCR:EQV Equivalent creep strain-2
EPTO:X, Y, Z ,XY,YZ,XZTotal 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, CreepStrain 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
γ13Transverse shear strain-Y
LOCI:X, Y, Z Integration point locations-5
SVAR:1, 2, ... , N State variables-6
ILSXZSXZ interlaminar shear stress-Y
ILSYZSYZ interlaminar shear stress-Y
ILSUMMagnitude of the interlaminar shear stress vector -Y
ILANGAngle of interlaminar shear stress vector (measured from the element x-axis toward the element y-axis in degrees)-Y
Sm: 11, 22, 12Membrane stresses-Y
Sb: 11, 22Bending stresses-Y
Sp: 11, 22, 12Peak stresses-Y
St: 13Averaged transverse shear stresses-Y
  1. The following stress solution repeats for top, middle, and bottom surfaces.

  2. 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.

  3. 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.

  4. Available only at centroid as a *GET item.

  5. Available only if OUTRES,LOCI is used.

  6. 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 NameETABLE and ESOL Command Input
ItemEIJ
N11SMISC1--
N22SMISC2--
N12SMISC3--
M11SMISC4--
M22SMISC5--
Q13SMISC6--
ε11SMISC7--
ε22SMISC8--
ε12SMISC9--
k11SMISC10--
k22SMISC11--
γ13SMISC12--
THICKSMISC13--
P1SMISC-1415
P2SMISC-1617
Sm: 11SMISC18--
Sm: 22SMISC19--
Sm: 12SMISC20--
Sb: 11SMISC21--
Sb: 22SMISC22--
Sp: 11 (at shell bottom)SMISC23--
Sp: 22 (at shell bottom)SMISC24--
Sp: 12 (at shell bottom)SMISC25--
Sp: 11 (at shell top)SMISC26--
Sp: 22 (at shell top)SMISC27--
Sp: 12 (at shell top)SMISC28--
St: 13SMISC29--
Output Quantity Name  ETABLE and ESOL Command Input
 Item Bottom of Layer i Top of Layer NL
ILSXZ SMISC 8 * (i - 1) + 318 * (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

SHELL208 Assumptions and Restrictions

  • 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.

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 Professional. 

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


Release 14.0 - © 2011 SAS IP, Inc. All rights reserved.