SHELL181 Element Description

SHELL181 is suitable for analyzing thin to moderately-thick shell structures. It is a four-node element with six degrees of freedom at each node: translations in the x, y, and z directions, and rotations about the x, y, and z-axes. (If the membrane option is used, the element has translational degrees of freedom only). The degenerate triangular option should only be used as filler elements in mesh generation.

SHELL181 is well-suited for linear, large rotation, and/or large strain nonlinear applications. Change in shell thickness is accounted for in nonlinear analyses. In the element domain, both full and reduced integration schemes are supported. SHELL181 accounts for follower (load stiffness) effects of distributed pressures.

SHELL181 can 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 SHELL181 for more details about this element.

SHELL181 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 four nodes (I, J, K, and L).

Figure 181.1:   SHELL181 Geometry

x₀ = Element x axis if element orientation (ESYS) is not specified.

x = Element x axis if element orientation is specified.

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 equal distance 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

When KEYOPT(11) = 0, 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 and is shown as x_o in Figure 181.1:  SHELL181 Geometry. In the most general case, the axis can be defined as:

where:

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

If edges IJ and KL are parallel (rectangular or trapezoidal elements), the default orientation is the same as described in Coordinate Systems (the first surface direction is aligned with the IJ side). For elements with nonparallel edges IJ and JK, the default orientation represents the stress state better because the element uses a single point of quadrature (by default) in the element domain.

With KEYOPT(11) = 1, the default element coordinate x₀ axis is directed from node I to node J. The z₀ axis is normal to the shell surface, and the y₀ axis is perpendicular to the x₀ and z₀ axes.

The default element orientation can be rotated by angle θ (in degrees) for the layer (SECDATA). 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. 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 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, SHELL181 provides stress and strain output at the center of the layer.

SHELL181 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 program chooses an appropriate penalty stiffness by default. A drill stiffness factor can be specified via the SECCONTROL command.

Element loads are described in Nodal Loading. Pressures can be input as surface loads on the element faces as shown by the circled numbers on Figure 181.1:  SHELL181 Geometry. 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 can 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.

Using KEYOPT(3), SHELL181 supports uniform reduced integration and full integration with incompatible modes. By default, this element uses the uniform reduced integration for performance reasons in nonlinear applications.

Using reduced integration with hourglass control creates some usage restrictions, although minimal. For example, to capture the in-plane bending of a cantilever or a stiffener (see Figure 181.2: SHELL181 Typical Bending Applications), a number of elements through the thickness direction is necessary. The performance gains achieved by using uniform reduced integration are significant enough to offset the need to use more elements. In relatively well-refined meshes, hourglassing issues are largely irrelevant.

When the reduced integration option is used, you can check the accuracy of the solution by comparing the total energy (SENE label in ETABLE) and the artificial energy (AENE label in ETABLE) introduced by hourglass control. If the ratio of artificial energy to total energy is less than 5%, the solution is generally acceptable. The total energy and artificial energy can also be monitored by using OUTPR,VENG in the solution phase.

Bilinear elements, when fully integrated, are too stiff in in-plane bending.SHELL181 uses the method of incompatible modes to enhance the accuracy in bending-dominated problems. This approach is also called "extra shapes" or "bubble" modes approach. SHELL181 uses the formulation that ensures satisfaction of the patch test (J. C. Simo and F. Armero, "Geometrically nonlinear enhanced strain mixed methods and the method of incompatible modes," IJNME, Vol. 33, pp. 1413-1449, 1992).

When including incompatible modes in the analysis, you must use full integration. KEYOPT(3) = 2 implies the inclusion of incompatible modes and the use of full (2x2) quadrature.

SHELL181, with KEYOPT(3) = 2 specified, does not have any spurious energy mechanisms. This specific form of SHELL181 is highly accurate, even with coarse meshes. Use KEYOPT(3) = 2 if you encounter any hourglass-related difficulties with the default options. KEYOPT(3) = 2 is also necessary if the mesh is coarse and in-plane bending of the elements dominate the response. We recommend this option with all layered applications.

KEYOPT(3) = 2 imposes the fewest usage restrictions. You can always choose this option. However, you can improve element performance by choosing the best option for your problem. Consider the problems illustrated in Figure 181.2: SHELL181 Typical Bending Applications

The cantilever beam and the beam cross-section to be modeled with shells are typical examples of in-plane bending-dominated problems. The use of KEYOPT(3) = 2 is the most effective choice in these circumstances. Reduced integration would require refined meshes. For example, reduced integration for the cantilever beam problem requires four elements through the thickness, whereas the full integration with incompatible modes only requires one element through the thickness.

For the stiffened shell, the most effective choice is to use KEYOPT(3) = 0 for the shell and KEYOPT(3) = 2 for the stiffener.

When KEYOPT(3) = 0 is specified, SHELL181 uses an hourglass control method for membrane and bending modes. By default, SHELL181 calculates the hourglass parameters for both metal and hyperelastic applications. To specify the hourglass stiffness scaling factors, use the SECCONTROL command.

When KEYOPT(5) = 1, the element uses an advanced formulation that incorporates initial curvature effects. The calculation for effective shell curvature change accounts for both shell-membrane and thickness strains. The 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, or in thick shell structures with unbalanced laminate construction or with shell offsets. The initial curvature of each element is calculated from the nodal shell normals. The shell normal at each node is obtained by averaging the shell normals from the surrounding SHELL181 elements. A coarse or highly distorted shell mesh can lead to significant error in the recovered element curvature; therefore, this option should be used with a smooth, adequately refined mesh only. To ensure proper representation of the original mesh, a nodal normal is replaced by the element shell normal in the curvature calculation if the subtended angle between these two is greater than 25 degrees.

When KEYOPT(5) = 2, a simplified curved-shell formulation is adopted. Unlike the advanced curved-shell formulation (KEYOPT(5) =1), the curvature effects in the shell offset handling are ignored. The simplified formulation generally leads to more robust nonlinear convergence.

SHELL181 includes the linear effects of transverse shear deformation. An assumed shear strain formulation of Bathe-Dvorkin is used to alleviate shear locking. The transverse shear stiffness of the element is a 2x2 matrix as shown below:

Transverse shear effects are not included in the normal material constitutive modeling for this element.

To define transverse shear stiffness values, issue the SECCONTROL command.

Transverse shear-correction factors k are calculated once at the start of the analysis for each section. The material properties used to evaluate the transverse shear correction factors are at the current reference temperature during solution. User-field variables and frequency are all set to zero when evaluating the material properties used to calculate the transverse shear correction factors.

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

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

SHELL181 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), and NLISO (nonlinear isotropic hardening) options. The kinematic hardening plasticity models can be invoked with BKIN (bilinear 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, the program 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 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.

With reduced integration and hourglass control (KEYOPT(3) = 0), low frequency spurious modes can appear if the mass matrix employed is not consistent with the quadrature rule. SHELL181 uses a projection scheme that effectively filters out the inertia contributions to the hourglass modes of the element. To be effective, a consistent mass matrix must be used. We recommend setting LUMPM,OFF for a modal analysis using this element type. The lumped mass option can, however, be used with the full integration options (KEYOPT(3) = 2).

KEYOPT(8) = 2 stores 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.

KEYOPT(9) = 1 reads 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. The pressure must be applied directly to the shell, and not via surface elements (SURFnnn).

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

A summary of the element input is given in "SHELL181 Input Summary". A general description of element input is given in Element Input.

SHELL181 Output Data

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

Several items are illustrated in Figure 181.3:  SHELL181 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 POST1. 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).

The program calculates 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:

SHELL181 does not support extensive basic element printout. POST1 provides more comprehensive output processing tools; therefore, ANSYS suggests using the OUTRES command to ensure that the required results are stored in the database.

Figure 181.3:   SHELL181 Stress Output

x0 = Element x axis if element orientation (ESYS) is not specified. (See KEYOPT(11).)

x = Element x axis if element orientation is specified.

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 181.2: SHELL181 Item and Sequence Numbers lists output available through ETABLE using the Sequence Number method. See Creating an Element Table and The Item and Sequence Number Table in this reference for more information. The following notation is used in Table 181.2: SHELL181 Item and Sequence Numbers:

SHELL181 Assumptions and Restrictions

SHELL181 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 

ANSYS Mechanical Premium