SOLSH190 Element Description

SOLSH190 is used for simulating shell structures with a wide range of thickness (from thin to moderately thick). The element possesses the continuum solid element topology and features eight-node connectivity with three degrees of freedom at each node: translations in the nodal x, y, and z directions. Thus, connecting SOLSH190 with other continuum elements requires no extra efforts. A degenerate prism option is available, but should only be used as filler elements in mesh generation. The element has plasticity, hyperelasticity, stress stiffening, creep, large deflection, and large strain capabilities. It also has mixed u-P formulation capability for simulating deformations of nearly incompressible elastoplastic materials, and fully incompressible hyperelastic materials. The element formulation is based on logarithmic strain and true stress measures.

You can use SOLSH190 for layered applications such as modeling laminated shells or sandwich construction. The layered section definition is given by section (SECxxx) commands. Accuracy in modeling composite shells is governed by the first-order shear-deformation theory (also known as Mindlin-Reissner shell theory).

See SOLSH190 for more details about this element.

Figure 190.1:  SOLSH190 Geometry

x_o = Element x-axis if ESYS is not supplied.

x = Element x-axis if ESYS is supplied.

SOLSH190 Input Data

The geometry, node locations, and the element coordinate system for this element are shown in Figure 190.1: SOLSH190 Geometry. The element is defined by eight nodes. The element coordinate system follows the shell convention where the z axis is normal to the surface of the shell. The node ordering must follow the convention that the I-J-K-L and M-N-O-P element faces represent the bottom and top shell surfaces, respectively. You can change the orientation within the plane of the layers via the ESYS command as you would for shell elements (as described in Coordinate Systems). To achieve the correct nodal ordering for a volume mapped (hexahedron) mesh, you can use the VEORIENT command to specify the desired volume orientation before executing the VMESH command. Alternatively, you can use the EORIENT command after automatic meshing to reorient the elements to be in line with the orientation of another element, or to be as parallel as possible to a defined ESYS axis.

Layered Section Definition Using Section Commands

You can associate SOLSH190 with a shell section (SECTYPE). The layered composite specifications (including layer thickness, material, orientation, and number of integration points through the thickness of the layer) are specified via shell section (SECxxx) commands. You can use the shell section commands even with a single-layered SOLSH190 element. The program obtains the actual layer thicknesses used for element calculations by scaling the input layer thickness so that they are consistent with the thickness between the nodes.

You can designate the number of integration points (1, 3, 5, 7, or 9) located through the thickness of each layer. Two points are located on the top and bottom surfaces respectively and the remaining points are distributed equal distance between the two points. The element requires at least two points through the entire thickness. When no shell section definition is provided, the element is treated as single-layered and uses two integration points through the thickness.

SOLSH190 does not support real constant input for defining layer sections.

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 and is shown as x_o in Figure 190.1: SOLSH190 Geometry. The axis can be defined as shown:

where:

{x}I, {x}J, . . . , {x}P = 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.

You can reorient the default first surface direction S1 in the element reference plane via the ESYS command. You can further rotate S1 by angle THETA (in degrees) for each layer via the SECDATA command to create layer-wise coordinate systems. See Coordinate Systems for details.

Element loads are described in Nodal Loading. Pressures may be input as surface loads on the element faces as shown by the circled numbers on Figure 190.1: SOLSH190 Geometry. Positive pressures act into the element.

If you specify no element body load for defining temperatures--that is, you define temperatures with commands other than BFE--SOLSH190 adopts an element-wise temperature pattern and requires only eight temperatures for the eight element nodes. Unspecified nodal temperatures default to the assigned uniform temperature (TUNIF). ANSYS computes all layer interface temperatures by interpolating nodal temperatures T1 ~ T8.

Alternatively, you can input temperatures as element body loads at the corners of the outside faces of the element and at the corners of the interfaces between layers. In such a case, the element uses a layer-wise pattern. Temperatures T1, T2, T3, T4 are used for the bottom of layer 1, temperatures T5, T6, T7, T8 are used for interface corners between layers 1 and 2, and so on between successive layers, ending with temperatures at the top layer NL. If you input exactly NL + 1 temperatures, 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. The first corner temperature T1 defaults to TUNIF. If all other corner temperatures are unspecified, they default to T1. For any other input pattern, unspecified temperatures default to TUNIF.

You can use the MP command to define the isotropic or orthotropic elastic material properties and the TB,ANEL command to define anisotropic elastic material properties. Other material properties include density, damping ratios, and coefficients of thermal expansion. You may also use the TB command to define nonlinear material behavior such as plasticity, hyperelasticity, viscoelasticity, creep, and viscoplasticity.

KEYOPT(2) = 1 activates the internal strain enhancements to the element transverse-shear strains. With this option, the element is capable of quadratic transverse-shear strain distributions through the entire thickness of the element. At least three integration points through the thickness are required for this option. Use a shell section to define more integration points through the thickness.

KEYOPT(6) = 1 sets the element for using u-P mixed formulation. For details on the use of mixed formulation, see Applications of Mixed u-P Formulations.

KEYOPT(16) = 1 activates steady state analysis (defined via the SSTATE command). For more information, see Steady State Rolling in the Mechanical APDL Theory Reference.

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.

"SOLSH190 Input Summary" contains a summary of element input. For a general description of element input, see Element Input.

SOLSH190 Output Data

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

Several items are illustrated in Figure 190.2: SOLSH190 Stress Output. See Element Table for Variables Identified By Sequence Number and The Item and Sequence Number Table in this reference for more information.

Figure 190.2:  SOLSH190 Stress Output

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

x = Element x-axis if ESYS is supplied.

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 1 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 view results.

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 190.2: SOLSH190 Item and Sequence Numbers lists output available through ETABLE using the Sequence Number method. See Element Table for Variables Identified By Sequence Number and The Item and Sequence Number Table in this reference for more information. The following notation is used in Table 190.2: SOLSH190 Item and Sequence Numbers:

SOLSH190 Assumptions and Restrictions

SOLSH190 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