8-Node Structural Shell
MP ME ST PR PRN DS DSS <> <> <> <> PP <> EME MFS

SHELL281 Element Description

SHELL281 is suitable for analyzing thin to moderately-thick shell structures. The element has eight nodes 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.)

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 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).

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.

See SHELL281 in the Mechanical APDL Theory Reference for more details about this element.

SHELL281 Input Data

The following figure shows the geometry, node locations, and the element coordinate system for this element. The element is defined by shell section information and 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 more 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.

Figure 281.1  SHELL281 Geometry

SHELL281 Geometry

xo = Element x-axis if element orientation (ESYS) is not provided.

x = Element x-axis if element orientation is provided.

Single-Layer Definition

To define the thickness (and other information), use section definition, as follows:


A single-layer shell section definition provides flexible options. For example, you can specify the number of integration points used and the material orientation.

Multilayer Definition

The shell section commands allow for layered shell definition. Options are available for specifying the thickness, material, orientation, and number of integration points through the thickness of the layers.

You can 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. The default number of integration points for each layer is three; however, when a single layer is defined and plasticity is present, the number of integration points is changed to a minimum of five during solution.

The following additional capabilities are available when defining shell layers:

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 four in-plane integration points:

Where element geometry {x} is given as follows:

(s,r) = two isoparametric element coordinates
hI (s,r) = shape functions associated with eight element nodes (see Mechanical APDL Theory Reference for more details)
{x}i = global coordinates of eight element nodes

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 θ (in degrees) for the layer via the SECDATA command. For an element, you can specify a single value of orientation in the plane of the element. Layer-wise orientation is supported.

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

The element supports degeneration into a triangular form. For better accuracy, however, ANSYS, Inc. recommends quadrilateral shaped elements. 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 Mechanical APDL Theory Reference), 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-layer shells. Irrespective of other settings, SHELL281 provides stress and strain output at the four in-plane integration points of the layer.

SHELL281uses 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 program chooses an appropriate penalty stiffness by default. A drill stiffness factor can be specified via the SECCONTROLS command.

Element loads are described in Nodal Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers in Figure 281.1. Positive pressures act into the element. Because shell edge pressures are input on a per-unit-length basis, per-unit-area quantities must be multiplied by the shell thickness.

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. 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:

To define transverse shear stiffness values, use the SECCONTROLS command .

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.

Use the BETAD command to specify the global value of damping. If MP,BETD is defined for the material number of the element (assigned with the MAT command), it is summed with 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.

SHELL281 uses an advanced shell formulation that accurately incorporates initial curvature effects. The calculation for effective shell curvature change accounts for both shell-membrane and thickness strains. The new formulation generally offers improved accuracy in curved shell structure simulations, especially when thickness strain is significant or the material anisotropy in the thickness direction cannot be ignored.

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.

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


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

Degrees of Freedom


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

Material Properties

Specify BETD 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
Birth and death
Element technology autoselect
Initial state
Large deflection
Large strain
Linear perturbation
Nonlinear stabilization
Section definition for layered shells and preintegrated general shell sections for input of homogenous section stiffnesses
User-defined material
Viscoplasticity / Creep

Element stiffness:

0 -- 

Bending and membrane stiffness (default)

1 -- 

Membrane stiffness only

2 -- 

Stress/strain evaluation only


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). (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


User thickness option:

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

SHELL281 Output Data

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

Several items are illustrated in Figure 281.2.

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).

ANSYS computes moments (M11, M22, M12) 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:

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

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 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 281.1  SHELL281 Element Output Definitions

ELElement number and nameYY
NODESNodes - I, J, K, L-Y
MATMaterial number-Y
THICKAverage thickness-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:1, 2, 3Principal stresses-1
S:INTStress intensity-1
S:EQVEquivalent stress-1
EPEL:X, Y, Z, XYElastic strains31
EPEL:EQVEquivalent elastic strains [7]-1
EPTH:X, Y, Z, XYThermal strains31
EPTH:EQVEquivalent thermal strains [7]-1
EPPL:X, Y, Z, XYAverage plastic strains32
EPPL:EQVEquivalent plastic strains [7]-2
EPCR:X, Y, Z, XYAverage creep strains32
EPCR:EQVEquivalent creep strains [7]-2
EPTO:X, Y, Z, XYTotal mechanical strains (EPEL + EPPL + EPCR)3-
EPTO:EQVTotal equivalent mechanical strains (EPEL + EPPL + EPCR)--
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 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, 12Membrane stresses-Y
Sb: 11, 22, 12Bending stresses-Y
Sp: 11, 22, 12Peak stresses-Y
St: 13, 23Averaged 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.

  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 281.2: 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 281.2: SHELL281 Item and Sequence Numbers:


output quantity as defined in the Table 181.1: SHELL181 Element Output Definitions


predetermined Item label for ETABLE


sequence number for single-valued or constant element data


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

Table 281.2  SHELL281 Item and Sequence Numbers

Output Quantity NameETABLE and ESOL Command Input
Sm: 11SMISC34----
Sm: 22SMISC35----
Sm: 12SMISC36----
Sb: 11SMISC37----
Sb: 22SMISC38----
Sb: 12SMISC39----
Sp: 11 (at shell bottom)SMISC40----
Sp: 22 (at shell bottom)SMISC41----
Sp: 12 (at shell bottom)SMISC42----
Sp: 11 (at shell top)SMISC43----
Sp: 22 (at shell top)SMISC44----
Sp: 12 (at shell top)SMISC45----
St: 13SMISC46----
St: 23SMISC47----
Output Quantity Name  ETABLE and ESOL Command Input
 Item Bottom 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

  • ANSYS recommends against using this element in triangular form, except as a filler element. Avoid triangular form especially in areas with high stress gradients.

  • Zero-area elements are not allowed. (Zero-area elements occur most often whenever the elements are numbered improperly.)

  • 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.

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

  • 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 and 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.

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

  • Before using this element in a simulation containing curved thick shell structures with unbalanced laminate construction or shell offsets, validate the usage via full 3-D modeling with a solid element in a simpler representative model. This element may underestimate the curved thick shell stiffness, particularly when the offset is large and the structure is under torsional load.

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

  • 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 via 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).

  • 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 has no bending stiffness, a condition that can result in solver and convergence problems.

SHELL281 Product Restrictions

ANSYS Professional. 

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

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