www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS



SHELL281

8-Node Finite Strain Shell

MP ME ST PR PRN DS DSS <> <> <> <> PP <>

Product Restrictions

SHELL281 Element Description

SHELL281 is suitable for analyzing thin to moderately-thick shell structures. It is an 8-node element with six degrees of freedom at each node: translations in the x, y, and z axes, and rotations about the x, y, and z-axes. (When using the membrane option, the element has translational degrees of freedom only.)

For better accuracy, ANSYS recommends quadrilateral shaped elements. Use degenerate triangular shapes sparingly.

SHELL281 is well-suited for linear, large rotation, and/or large strain nonlinear applications. Change in shell thickness is accounted for in nonlinear analyses. The element accounts for follower (load stiffness) effects of distributed pressures.

SHELL281 may be used for layered applications for modeling laminated composite shells or sandwich construction. The accuracy in modeling composite shells is governed by the first order shear deformation theory (usually referred to as Mindlin-Reissner shell theory).

SHELL281 can be used instead of SHELL91, SHELL93, and SHELL99 for most problems.

Figure 281.1  SHELL281 Geometry

xo = Element x-axis if ESYS is not provided.

x = Element x-axis if ESYS is provided.

SHELL281 Input Data

The geometry, node locations, and the element coordinate system for this element are shown in Figure 281.1: "SHELL281 Geometry". The element is defined by eight nodes: I, J, K, L, M,N, O and P. Midside nodes may not be removed from this element. See Quadratic Elements (Midside Nodes) in the Modeling and Meshing Guide for additional information about the use of midside nodes. A triangular-shaped element may be formed by defining the same node number for nodes K, L and O. The element formulation is based on logarithmic strain and true stress measures. The element kinematics allow for finite membrane strains (stretching). However, the curvature changes within a time increment are assumed to be small. To define the thickness and other information, you can use either real constants or section definition (and a section can be partially defined using data from a FiberSIM .xml file). The option of using real constants is available only for single-layer shells. If a SHELL281 element references both real constant set data and a valid shell section type, real constant data is ignored.

SHELL281 also accepts the preintegrated shell section type (SECTYPE,,GENS). When the element is associated with the GENS section type, thickness or material definitions are not required. For more information, see Using Preintegrated General Shell Sections.

Thickness Definition Using Real Constants

The thickness of the shell may be defined at each of its nodes. The thickness is assumed to vary smoothly over the area of the element. If the element has a constant thickness, only TK(I) needs to be input. If the thickness is not constant, all four thicknesses must be input.

Layered Section Definition Using Section Commands

Alternatively, the shell thickness and more general properties may be specified using section commands. SHELL281 may be associated with a shell section (SECTYPE). Shell section is a more general method to define shell construction than the real constants option. Shell section commands allow for layered composite shell definition, and provide the input options for specifying the thickness, material, orientation and number of integration points through the thickness of the layers. Note that a single layer shell is not precluded using shell section definition, but provides more flexible options such as the use of the ANSYS function builder to define thickness as a function of global coordinates and the number of integration points used.

You may designate the number of integration points (1, 3, 5, 7, or 9) located through the thickness of each layer when using section input. When only one, the point is always located midway between the top and bottom surfaces. If three or more points, two points are located on the top and bottom surfaces respectively and the remaining points are distributed at equal distances between the two points. An exception occurs when designating five points, where the quarter point locations are moved five percent toward their nearest layer surface to agree with the locations selected with real constant input. The default number of integration points for each layer is 3. However, when a single layer is defined and plasticity is present, the number of integration points will be changed to a minimum of 5 during solution. Note that when Real Constants are used, ANSYS uses 5 points of integration and Sections will produce a comparable solution.

Other Input

The default orientation for this element has the S1 (shell surface coordinate) axis aligned with the first parametric direction of the element at the center of the element, which connects the midsides of edges LI and JK. In the most general case, the axis can be defined as:

where:

{x}I, {x}J, {x}K, {x}L = global nodal coordinates

For undistorted elements, the default orientation is the same as described in Coordinate Systems (the first surface direction is aligned with the IJ side).

The first surface direction S1 can be rotated by angle THETA (in degrees) as a real constant for the element or for using the SECDATA command. For an element, you can specify a single value of orientation in the plane of the element. Layer-wise orientation is possible when section definition is used.

You can also define element orientation via the ESYS command. For more information, see Coordinate Systems.

The element supports degeneration into a triangular form; however, use of the triangular form is not recommended, except when used as mesh filler elements or with the membrane option (KEYOPT(1) = 1). The triangle form is generally more robust when using the membrane option with large deflections.

To evaluate stresses and strains on exterior surfaces, use KEYOPT(1) = 2. When used as overlaid elements on the faces of 3-D elements, this option is similar to the surface stress option (described in the Theory Reference for ANSYS and ANSYS Workbench), but is more general and applicable to nonlinear analysis. The element used with this option does not provide any stiffness, mass, or load contributions. This option should only be used in single-layered shells. Irrespective of other settings, SHELL181 provides stress and strain output at the four in-plane integration points of the layer.

SHELL281 uses a penalty method to relate the independent rotational degrees of freedom about the normal (to the shell surface) with the in-plane components of displacements. The ANSYS program chooses an appropriate penalty stiffness by default; however, you can change the default value if necessary via the tenth real constant (drill stiffness factor). The value of this real constant is the scaling parameter for the default penalty stiffness. Using a higher value could contribute to a larger nonphysical energy content in the model; therefore, use caution when changing the default. When using the section definition with SHELL281, drill stiffness factor may be specified via the SECCONTROLS command.

Element loads are described in Node and Element Loads. Pressures may be input as surface loads on the element faces as shown by the circled numbers in Figure 281.1: "SHELL281 Geometry". Positive pressures act into the element. Edge pressures are input as force per unit length.

Temperatures may be input as element body loads at the corners of the outside faces of the element and at the corners of the interfaces between layers (1-1024 maximum). The first corner temperature T1 defaults to TUNIF. If all other temperatures are unspecified, they default to T1. If KEYOPT(1) = 0 and if exactly NL+1 temperatures are input, one temperature is used for the four bottom corners of each layer, and the last temperature is used for the four top corner temperatures of the top layer. If KEYOPT(1) = 1 and if exactly NL temperatures are input, one temperature is used for the four corners of each layer. That is, T1 is used for T1, T2, T3, and T4; T2 (as input) is used for T5, T6, T7, and T8, etc. For any other input pattern, unspecified temperatures default to TUNIF.

SHELL281 includes the effects of transverse shear deformation. The transverse shear stiffness of the element is a 2x2 matrix as shown below:

In the above matrix, R7, R8, and R9 are real constants 7, 8, and 9. (See Table 281.1: "SHELL281 Real Constants".) You can override the default transverse shear stiffness values by assigning different values to those real constants. This option is effective for analyzing sandwich shells. Alternatively, the SECCONTROLS command you to define transverse shear stiffness values.

For a single-layer shell with isotropic material, default transverse shear stiffnesses are:

In the above matrix, k = 5/6, G = shear modulus, and h = thickness of the shell.

SHELL281 can be associated with linear elastic, elastoplastic, creep, or hyperelastic material properties. Only isotropic, anisotropic, and orthotropic linear elastic properties can be input for elasticity. The von Mises isotropic hardening plasticity models can be invoked with BISO (bilinear isotropic hardening), MISO (multilinear isotropic hardening), and NLISO (nonlinear isotropic hardening) options. The kinematic hardening plasticity models can be invoked with BKIN (bilinear kinematic hardening), MKIN and KINH (multilinear kinematic hardening), and CHABOCHE (nonlinear kinematic hardening). Invoking plasticity assumes that the elastic properties are isotropic (that is, if orthotropic elasticity is used with plasticity, ANSYS assumes the isotropic elastic modulus = EX and Poisson's ratio = NUXY).

Hyperelastic material properties (2, 3, 5, or 9 parameter Mooney-Rivlin material model, Neo-Hookean model, Polynomial form model, Arruda-Boyce model, and user-defined model) can be used with this element. Poisson's ratio is used to specify the compressibility of the material. If less than 0, Poisson's ratio is set to 0; if greater than or equal to 0.5, Poisson's ratio is set to 0.5 (fully incompressible).

Both isotropic and orthotropic thermal expansion coefficients can be input using MP,ALPX. When used with hyperelasticity, isotropic expansion is assumed.

Issue the BETAD command to specify the global value of damping. If MP,DAMP is defined for the material number of the element (assigned with the MAT command), it is used for the element instead of the value from the BETAD command. Similarly, use the TREF command to specify the global value of reference temperature. If MP,REFT is defined for the material number of the element, it is used for the element instead of the value from the TREF command. But if MP,REFT is defined for the material number of the layer, it is used instead of either the global or element value.

KEYOPT(8) = 2 is used 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. 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.

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

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.

You can apply an initial stress state to this element via the INISTATE command. For more information, see the INISTATE command, and also Initial Stress Loading in the Basic Analysis Guide. Alternately, you can set KEYOPT(10) = 1 to read initial stresses from the user subroutine USTRESS. For details on user subroutines, see the Guide to ANSYS User Programmable Features.

A summary of the element input is given in "SHELL281 Input Summary". A general description of element input is given in Element Input.

SHELL281 Input Summary

Nodes

I, J, K, L, M, N, O, P

Degrees of Freedom

UX, UY, UZ, ROTX, ROTY, ROTZ if KEYOPT(1) = 0

UX, UY, UZ if KEYOPT(1) = 1

Real Constants
TK(I), TK(J), TK(K), TK(L), THETA, ADMSUA
E11, E22, E12, DRILL
See Table 281.1: "SHELL281 Real Constants" for more information.
If a SHELL281 element references a valid shell section type, any real constant data specified is ignored.
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

Specify DAMP only once for the element (use MAT command to assign material property set). REFT may be provided once for the element, or may be assigned on a per layer basis. See the discussion in "SHELL281 Input Summary" for more details.

Surface Loads
Pressures -- 
face 1 (I-J-K-L) (bottom, in +N direction),
face 2 (I-J-K-L) (top, in -N direction),
face 3 (J-I), face 4 (K-J), face 5 (L-K), face 6 (I-L)
Body Loads
Temperatures -- 

For KEYOPT(1) = 0 (Bending and membrane stiffness):

T1, T2, T3, T4 (at bottom of layer 1), T5, T6, T7, T8 (between layers 1-2); similarly for between next layers, ending with temperatures at top of layer NL(4*(NL+1) maximum). Hence, for one-layer elements, eight temperatures are used.

For KEYOPT(1) = 1 (Membrane stiffness only):

T1, T2, T3, T4 for layer 1, T5, T6, T7, T8 for layer 2, similarly for all layers (4*NL maximum). Hence, for one-layer elements, four temperatures are used.

Special Features
Plasticity (PLASTIC, BISO, MISO, NLISO, BKIN, MKIN, KINH, CHABOCHE, HILL)
Hyperelasticity (AHYPER, HYPER)
Viscoelasticity (PRONY, SHIFT)
Viscoplasticity/Creep (CREEP, RATE)
Elasticity (ANEL)
Other material (USER, SDAMP)
Stress stiffening
Large deflection
Large strain
Initial stress import
Nonlinear stabilization
Automatic selection of element technology
Birth and death
Section definition for layered shells and preintegrated shell sections for input of homogenous section stiffnesses

Note

Items in parentheses refer to data tables associated with the TB command. See the Theory Reference for ANSYS and ANSYS Workbench for details about the material models.

Note

See Automatic Selection of Element Technologies and ETCONTROL for more information on selection of element technologies.

KEYOPT(1)

Element stiffness:

0 -- 

Bending and membrane stiffness (default)

1 -- 

Membrane stiffness only

2 -- 

Stress/strain evaluation only

KEYOPT(8)

Specify layer data storage:

0 -- 

Store data for bottom of bottom layer and top of top layer (multi-layer elements) (default)

1 -- 

Store data for TOP and BOTTOM, for all layers (multi-layer elements)

Note

The volume of data may be considerable.

2 -- 

Store data for TOP, BOTTOM, and MID for all layers; applies to single- and multi-layer elements

KEYOPT(9)

User thickness option:

0 -- 

No user subroutine to provide initial thickness (default)

1 -- 

Read initial thickness data from user subroutine UTHICK

Note

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

KEYOPT(10)

User-defined initial stress:

0 -- 

No user subroutine to provide initial stress (default)

1 -- 

Read initial stress data from user subroutine USTRESS

Note

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

Table 281.1  SHELL281 Real Constants

No.NameDescription
1TK(I)Thickness at node I
2TK(J)Thickness at node J
3TK(K)Thickness at node K
4TK(L)Thickness at node L
5THETAAngle of first surface direction, in degrees
6ADMSUAAdded mass per unit area
7E11Transverse shear stiffness[2]
8E22Transverse shear stiffness[2]
9E12Transverse shear stiffness[2]
10Drill Stiffness FactorIn-plane rotation stiffness[1,2]
11Membrane HG FactorMembrane hourglass control factor[1,2]
12Bending HG FactorBending hourglass control factor[1,2]
  1. Valid values for these real constants are any positive number. However, we recommend using values between 1 and 10. If you specify 0.0, the value defaults to 1.0.

  2. ANSYS provides default values.

*See SECCONTROLS command if section definition is used.

SHELL281 Output Data

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

Several items are illustrated in Figure 281.2: "SHELL281 Stress Output".

KEYOPT(8) controls the amount of data output to the results file for processing with the LAYER command. Interlaminar shear stress is available as SYZ and SXZ evaluated at the layer interfaces. KEYOPT(8) must be set to either 1 or 2 to output these stresses in the POST1 postprocessor. A general description of solution output is given in Solution Output. See the Basic Analysis Guide for ways to review 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 forces Q13, Q23 are available only in resultant form: that is, use SMISC,7 (or 8). Likewise, the transverse shear strains, γ13 and γ23, are constant through the thickness and are only available as SMISC items (SMISC,15 and SMISC,16, respectively).

SHELL281 does not support extensive basic element printout. POST1 provides more comprehensive output processing tools; therefore, ANSYS suggests issuing the OUTRES command to ensure that the required results are stored in the database.

Figure 281.2  SHELL281 Stress Output

xo = Element x-axis if ESYS is not provided.
x = Element x-axis if ESYS is provided.

The Element Output Definitions table uses the following notation:

A colon (:) in the Name column indicates 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 a - indicates that the item is not available.

Table 281.2  SHELL281 Element Output Definitions

NameDefinitionOR
ELElement number and name-Y
NODESNodes - I, J, K, L-Y
MATMaterial number-Y
THICKAverage thickness-Y
VOLU:Volume-Y
XC, YC, ZCLocation where results are reported-4
PRESPressures P1 at nodes I, J, K, L; P2 at I, J, K, L; P3 at J,I; P4 at K,J; P5 at L,K; P6 at I,L-Y
TEMPT1, T2, T3, T4 at bottom of layer 1, T5, T6, T7, T8 between layers 1-2, similarly for between next layers, ending with temperatures at top of layer NL(4*(NL+1) maximum)-Y
LOCTOP, MID, BOT, or integration point location-1
S:X, Y, Z, XY, YZ, XZStresses31
S:INTStress intensity-1
S:EQVEquivalent stress-1
EPEL:X, Y, Z, XYElastic strains31
EPEL:EQVEquivalent elastic strains [7]31
EPTH:X, Y, Z, XYThermal strains31
EPTH:EQVEquivalent thermal strains [7]31
EPPL:X, Y, Z, XYAverage plastic strains32
EPPL:EQVEquivalent plastic strains [7]32
EPCR:X, Y, Z, XYAverage creep strains32
EPCR:EQVEquivalent creep strains [7]32
EPTO:X, Y, Z, XYTotal mechanical strains (EPEL + EPPL + EPCR)Y-
EPTO:EQVTotal equivalent mechanical strains (EPEL + EPPL + EPCR)Y-
NL:EPEQAccumulated equivalent plastic strain-2
NL:CREQAccumulated equivalent creep strain-2
NL:SRATPlastic yielding (1 = actively yielding, 0 = not yielding)-2
NL:PLWKPlastic work-2
NL:HPRESHydrostatic pressure-2
SEND:ELASTIC, PLASTIC, CREEPStrain energy densities-2
N11, N22, N12In-plane forces (per unit length)-Y
M11, M22, M12Out-of-plane moments (per unit length)-8
Q13, Q23Transverse shear forces (per unit length)-8
ε11, ε22, ε12Membrane strains-Y
k11, k22, k12Curvatures-8
γ13, γ23Transverse shear strains-8
LOCI:X, Y, ZIntegration point locations-5
SVAR:1, 2, ... , NState variables-6
ILSXZ SXZ interlaminar shear stress -Y
ILSYZ SYZ interlaminar shear stress -Y
ILSUM Interlaminar shear stress vector sum -Y
ILANG Angle of interlaminar shear stress vector (measured from the element x-axis toward the element y-axis in degrees) -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.

  3. Stresses, total strains, plastic strains, elastic strains, creep strains, and thermal strains in the element coordinate system are available for output (at all five 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 are used.

  7. The equivalent strains use an effective Poisson's ratio: for elastic and thermal this value is set by the user (MP,PRXY); for plastic and creep this value is set at 0.5.

  8. Not available if the membrane element option is used (KEYOPT(1) = 1).

Table 281.3: "SHELL281 Item and Sequence Numbers" lists output available through ETABLE using the Sequence Number method. See Creating an Element Table in the Basic Analysis Guide and The Item and Sequence Number Table in this document for more information. The following notation is used in Table 281.3: "SHELL281 Item and Sequence Numbers":

Name

output quantity as defined in the Table 181.2: "SHELL181 Element Output Definitions"

Item

predetermined Item label for ETABLE

E

sequence number for single-valued or constant element data

I,J,K,L

sequence number for data at nodes I, J, K, L

Table 281.3  SHELL281 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input
ItemEIJKL
N11SMISC1----
N22SMISC2----
N12SMISC3----
M11SMISC4----
M22SMISC5----
M12SMISC6----
Q13SMISC7----
Q23SMISC8----
ε11SMISC9----
ε22SMISC10----
ε12SMISC11----
k11SMISC12----
k22SMISC13----
k12SMISC14----
γ13SMISC15----
γ23SMISC16----
THICKSMISC17----
P1SMISC-18192021
P2SMISC-22232425
P3SMISC-2726--
P4SMISC--2928-
P5SMISC---3130
P6SMISC-32--33
Output Quantity Name ETABLE and ESOL Command Input
ItemBottom of Layer i Top of Layer NL
ILSXZ SMISC 8 * (i - 1) + 518 * (NL - 1) + 52
ILSYZ SMISC 8 * (i - 1) + 53 8 * (NL - 1) + 54
ILSUM SMISC 8 * (i - 1) + 55 8 * (NL - 1) + 56
ILANG SMISC 8 * (i - 1) + 57 8 * (NL - 1) + 58

SHELL281 Assumptions and Restrictions

  • Zero area elements are not allowed. (This condition occurs most often whenever the elements are not numbered properly.)

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

  • In a nonlinear analysis, the solution is terminated if the thickness at any integration point that was defined with a nonzero thickness vanishes (within a small numerical tolerance).

  • ANSYS, Inc.recommends against using SHELL281 in triangular form.

  • This element works best with a full Newton-Raphson solution scheme (NROPT,FULL,ON). For nonlinear problems dominated by large rotations and loading, ANSYS recommends against using the PRED,ON command.

  • 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.

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

  • 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.

  • Transverse shear stiffness of the shell section is estimated by a 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.

  • A maximum of 250 layers is supported.

  • The layer orientation angle has no effect if the material of the layer is hyperelastic.

  • If a shell section has only one layer and the number of section integration points is equal to one, or if KEYOPT(1) = 1, then the shell does not have any bending stiffness. In such a case, solver difficulties and convergence problems may occur.

  • Stress stiffening is always included in geometrically nonlinear analyses (NLGEOM,ON). It is ignored in geometrically linear analyses (NLGEOM,OFF) when specified via SSTIF,ON. Prestress effects can be activated via a PSTRES command.

  • The through-thickness stress, SZ, is always zero.

  • When the element is associated with preintegrated shell sections (SECTYPE,,GENS), additional restrictions apply. For more information, see Considerations for Employing Preintegrated Shell Sections.

  • This element does not support the RIMPORT command.

SHELL281 Product Restrictions

ANSYS Professional. 

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