REINF263 Element Description

Use REINF263 with standard 2-D solid and shell elements (referred to here as the base elements) to provide extra reinforcing to those elements.

The element uses a smeared approach and is suitable for modeling evenly spaced reinforcing fibers that appear in layered form. Each reinforcing layer contains a cluster of fibers with unique orientation, material, and cross-section area, and is simplified as a homogeneous membrane having unidirectional stiffness. You can specify multiple layers of reinforcing in one REINF263 element. The nodal locations, degrees of freedom, and connectivity of the REINF263 element are identical to those of the base element.

REINF263 has plasticity, stress stiffening, creep, large deflection, and large strain capabilities.

For more information, see Reinforcing in the Mechanical APDL Structural Analysis Guide.

Figure 263.1:  REINF263 Geometry

Figure 263.2:  REINF263 Coordinate System

X = Layer x-axis if layer orientation angle θ is specified (SECDATA,,,,THETA)

X0 = Layer x-axis if layer orientation angle θ is not specified

REINF263 Input Data

The geometry and nodal locations for this element are shown in Figure 263.1: REINF263 Geometry. The REINF263 element and its base element share the same nodes and element connectivity.

You can easily create REINF263 elements from the selected base elements via the EREINF command. Section commands (SECTYPE and SECDATA) define the material ID, cross-section area, spacing, location, and orientation of reinforcing fibers.

The equivalent thickness h of the smeared reinforcing layer is given by

where A is the cross-section area of a single fiber, and S is the distance between two adjacent fibers.

The coordinate systems for one reinforcing layer are shown in Figure 263.2: REINF263 Coordinate System. Each reinforcing layer is indicated by its intersection points (II, JJ for linear base elements, and II, JJ, KK, for quadratic base elements) with the base elements. Fibers in this layer are always parallel to the first coordinate axis x. The x axis is default to the first parametric direction S1 at the center of the layer. The default axis is defined as

where

You can reorient the layer coordinate system by angle θ (in degrees) for each layer. The value of θ is also provided for each layer via the SECDATA command. For more information about visualizing fiber orientations, see the /PSYMB command documentation.

You can use REINF263 to reinforce 2-D solid elements with plane stress, plane strain, axisymmetric (with or without torsion), and generalized plane strain behaviors. The element can also reinforce axisymmetric shells or membranes (with or without uniform torsion). The element accounts for various base element behaviors automatically.

REINF263 allows tension-only or compression-only reinforcing fibers. You can specify the desired fiber behavior (SECCONTROL).

The element can account for redundant base element material where the reinforcing fibers are located (SECCONTROL,,REMBASE).

The REINF263 element does not accept element loading. Apply element loading only to the base element. The temperature of the REINF263 element is identical to the temperature of the base element.

You can import an initial stress state for this element (INISTATE). For more information, see Initial State in the Mechanical APDL Advanced Analysis Guide.

A summary of the element input follows.

REINF263 Output Data

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

The following figure illustrates the axial stress component:

Figure 263.3:   REINF263 Stress Output

Unlike layered solid or shell elements (such as SHELL181), REINF263 always outputs the element solution for all reinforcing layers. You can select solution items for a specific reinforcing layer (LAYER) for listing and visualization by using full graphics (/GRAPHICS,FULL). Visualization via PowerGraphics (/GRAPHICS,POWER) is not affected by the LAYER command; all reinforcing layers are displayed simultaneously. See the Basic Analysis Guide for ways to review results.

To inspect REINF263 element results, select only REINF263 element results or adjust translucency level of the base elements before executing any plotting command. REINF263 display options are also available directly via the GUI (Main Menu> Preprocessor> Sections> Reinforcing> Display Options).

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 263.2: REINF263 Item and Sequence Numbers lists output available via ETABLE using the Sequence Number method. See Creating an Element Table and The Item and Sequence Number Table in this document for more information. The following notation is used in Table 263.2: REINF263 Item and Sequence Numbers:

The i value (where i = 1, 2, 3, ..., NL) represents the reinforcing layer number of the element. NL is the maximum reinforcing layer number.

REINF263 Assumptions and Restrictions

REINF263 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 Premium