REINF265 Element Description

The REINF265 3D smeared reinforcing element is available in two forms:

3-D Structural/Thermal Smeared Reinforcing Element Description

For a structural reinforcing analysis, use REINF265 with standard 3D solid and shell elements (referred to as the base elements) to provide extra reinforcing to those elements. For a thermal reinforcing analysis, the supported base elements are thermal solids SOLID278 and SOLID279, and SOLID291.

The element uses a smeared approach and is suitable for modeling homogeneous thin structures or evenly spaced reinforcing fibers that appear in layered form. When used for modeling reinforcing fibers, 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 or conductivity. You can specify multiple layers of reinforcing in one REINF265 element. The nodal locations, degrees of freedom, and connectivity of the REINF265 element are identical to those of the base element.

For discrete reinforcing modeling options, see the documentation for the REINF264 element.

REINF265 has plasticity, stress-stiffening, creep, large-deflection, and large-strain capabilities.

For more information, see Reinforcing and Direct Element Embedding in the Structural Analysis Guide.

Figure 265.1: REINF265 Structural/Thermal Geometry

3D 8-Node Solid or Solid Shell	3D 20-Node Solid
3D 10-Node Tetrahedral Solid	3D 4-Node Shell
3D 8-Node Shell

Figure 265.2: REINF265 Structural/Thermal Coordinate System

Uniaxial Stress State	Plane Stress State
X0 = Layer x axis if layer system LSYS and layer-orientation angle θ are not specified (default) Xc = Layer x axis if a local coordinate system for the layer is specified (SECDATA,,,KCN) Xf = Layer x axis if layer orientation angle θ is specified (SECDATA,,,,THETA)

REINF265 Structural/Thermal Input Data

The geometry and nodal locations for this element are shown in Figure 265.1: REINF265 Structural/Thermal Geometry. The REINF265 element and its base element share the same nodes and element connectivity.

You can easily create REINF265 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. See Reinforcing and Direct Element Embedding in the Structural Analysis Guide for more information about creating REINF265 elements.

Each reinforcing layer can contain a cluster of fibers with unique orientation, material, and cross-section area, simplified as a homogeneous membrane having unidirectional stiffness.

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.

REINF265 can also be used to model homogeneous reinforcing membranes. The spacing input S is ignored and always set to 1.0 for reinforcing membranes. Therefore, the thickness h is equal to the cross-section area input A.

For a structural analysis, REINF265 supports a plane-stress or uniaxial-stress state (SECCONTROL,,,MEMOPT). For a thermal analysis, MEMOPT controls thermal conductivity KYY in the member (individual reinforcing) coordinate system. If MEMOPT = 1, KYY = 0 and conduction is allowed only in the X direction. Select the plane-stress state for homogeneous reinforcing membranes, and the uniaxial-stress state for clusters of reinforcing fibers.

The coordinate systems for one reinforcing layer are shown in Figure 265.2: REINF265 Structural/Thermal Coordinate System. Each reinforcing layer is indicated by its intersection points (II, JJ, KK, LL for linear base elements, and II, JJ, KK, LL, MM, NN, OO, PP 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

{x}II, {x}JJ, {x}KK, {x}LL = global nodal coordinates

You can reorient the default layer coordinate system by projecting a local coordinate system (LOCAL) to the layer plane. One local coordinate system is allowed for each layer. The local coordinate system reference number is given via the SECDATA command.

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

For a structural analysis, REINF265 enables you to specify tension-only or compression-only reinforcing fiber behavior (SECCONTROL,TENSKEY). This option is not available when the plane-stress state is selected (SECCONTROL,,,MEMOPT).

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

The element can account for transverse shear stiffness when using the plane-stress state with transverse shear stiffness (SECCONTROL,,,2). When solid base elements are used, the element can also account for bending stiffness (SECCONTROL,,,3).

For a structural analysis, REINF265 allows body-force-density element loading (BFE), as shown in these examples:

If applying body-force density to REINF265 elements (BFE), the program applies a uniform load to all members in the element. You can apply non-uniform body-force density to individual members via the mesh-independent method by loading to MESH200 elements.

Apply other structural element loading only to the base element. The temperature of the REINF265 element is identical to the temperature of the base element in a structural analysis.

For thermal reinforcing analysis, REINF265 allows heat-generation (HGEN) element loading (BFE), as shown in these examples:

You can apply an initial state to this element in either of the following ways:

A summary of the element input follows.

REINF265 Structural/Thermal Output Data

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

The following figure illustrates the axial stress component:

Figure 265.3: REINF265 Structural or Thermal Output

Unlike layered solid or shell elements (such as SHELL181), REINF265 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.

REINF265 element solution is always output in the layer coordinate system and does not support transformation to a different coordinate system. RSYS has no effect on REINF265 element solution.

To inspect REINF265 element results, select only REINF265 element results or adjust translucency level of the base elements before executing any plotting command. REINF265 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 letter or number refers to a table footnote that describes when the item is conditionally available, and “-” indicates that the item is not available.

Table 265.3: REINF265 Structural/Thermal 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 document for more information. The following notation is used in Table 265.3: REINF265 Structural/Thermal Item and Sequence Numbers:

The i value (where i = 1, 2, 3, ..., NL) represents the reinforcing member number of the element. NL is the maximum reinforcing member number (1 NL 250).

REINF265 Structural/Thermal Assumptions and Restrictions

REINF265 Structural/Thermal Product Restrictions

No product-specific restrictions exist for this element.

3-D Special-Purpose Smeared Reinforcing Element Description

REINF265 can represent the interior intersection areas between embedded elements (elements completely or partially enclosed within other elements) and the base elements (elements surrounding the embedded elements). These special-purpose reinforcing elements capture the bonding stiffness between the embedded and base elements. However, they do not introduce additional structural stiffness, mass, and external forces in structural analyses, nor do they introduce additional conduction, damping, and external heat in a thermal analysis.

REINF265 special-purpose elements are generated via EEMBED.

In this figure, black lines and dots indicate a base element, blue lines and dots indicate an embedded beam element, and red lines indicate the interior intersection area represented by a REINF265 special-purpose element:

Figure 265.4: REINF265 Special-Purpose Geometry

3D 2-Node Beam with RECT section embedded in 3D 8-Node Solid	3D 2-Node Beam with RECT section embedded in 3D 20-Node Solid
3D 2-Node Beam with RECT section embedded in 3D 10-Node Solid

For more information, see Direct-Embedding Workflow in the Structural Analysis Guide.

REINF265 Special-Purpose Output Data

REINF265 elements generated via EEMBED have no solution output except nodal displacements (for structural analysis) or temperature (for thermal analysis).

REINF265 Special-Purpose Product Restrictions

No product-specific restrictions exist for this element.