Embedded Elements

The embedded element technique is used to specify that an element or group of elements is embedded in “host” elements. For example, the embedded element technique can be used to model rebar reinforcement. Abaqus searches for the geometric relationships between nodes of the embedded elements and the host elements. If a node of an embedded element lies within a host element, the translational degrees of freedom and pore pressure degree of freedom at the node are eliminated and the node becomes an “embedded node.” The translational degrees of freedom and pore pressure degree of freedom of the embedded node are constrained to the interpolated values of the corresponding degrees of freedom of the host element. Embedded elements are allowed to have rotational degrees of freedom, but these rotations are not constrained by the embedding. Multiple embedded element definitions are allowed.

Different element types can be used in the element set containing embedded elements and the element set containing the host elements. However, all the host elements can have only translational degrees of freedom and pore pressure degree of freedom. The number of translational degrees of freedom at a node on the embedded element must be identical to the number of translational degrees of freedom at a node on the host element. If elements of type FP2D2, FP3D2, FPC2D2, and FPC3D2 with only pore pressure degree of freedom are embedded in a host element that has both translational and pore pressure degrees of freedom, only the common pore pressure degree of freedom is constrained at the embedded node.

The following general types of “embedded elements-in-host elements” are provided:

• Two-dimensional models:

  • Beam-in-solid

  • Solid-in-solid

  • Truss-in-solid

  • Fluid pipe-in-solid

• Axisymmetric models:

  • Membrane-in-solid (Abaqus/Standard only)

  • Shell-in-solid

  • Solid-in-solid

  • Surface-in-solid (Abaqus/Standard only)

• Three-dimensional models:

  • Beam-in-solid

  • Membrane-in-solid

  • Shell-in-solid

  • Solid-in-solid

  • Surface-in-solid

  • Truss-in-solid

  • Fluid pipe-in-solid

By default, the elements in the vicinity of the embedded elements are searched for elements that contain embedded nodes; the embedded nodes are then constrained by the response of these host elements. To preclude certain elements from constraining the embedded nodes, you can define a host element set; the search will be limited to this subset of the host elements in the model. This feature is strongly recommended if the embedded nodes are close to discontinuities in the model (such as cracks and contact pairs).

EMBEDDED ELEMENT, HOST ELSET=name

Interaction module: Create Constraint: Embedded region: choose Select Region from the prompt area when selecting the host region

You must specify the embedded elements. Individual elements or element sets can be specified. By default, Abaqus issues an error message if it is unsuccessful in fully embedding all of the specified embedded elements into host elements. Optionally, you can allow partial embedding in which only those nodes of embedded elements within host elements will be constrained.

An embedded element may share some nodes with host elements. These nodes, however, will not be considered to be embedded nodes.

EMBEDDED ELEMENT, PARTIAL EMBED=NO
embedded elements

EMBEDDED ELEMENT, PARTIAL EMBED=YES
embedded elements

Interaction module: Create Constraint: Embedded region: select the embedded region

Optionally, you can specify the embedded nodes. Individual nodes or node sets can be specified. By default, Abaqus issues an error message if it is unsuccessful in fully embedding all of the specified embedded nodes into host elements.

EMBEDDED ELEMENT, EMBED NODES
embedded nodes

A geometric tolerance is used to define how far an embedded node can lie outside the regions of the host elements in the model. By default, embedded nodes must lie within a distance calculated by multiplying the average size of all non-embedded elements in the model by 0.05; however, you can change this tolerance.

You can define the geometric tolerance as a fraction of the average size of all non-embedded elements in the model. Alternatively, you can define the geometric tolerance as an absolute distance in the length units chosen for the model. If you specify both exterior tolerances, Abaqus uses the tighter tolerance of the two. The average size of all the non-embedded elements is calculated and multiplied by the fractional exterior, which is then compared to the absolute exterior tolerance to determine the tighter tolerance of the two. The exterior tolerance for embedded elements in host elements is indicated by the shaded region in Figure 1.

Figure 1. The exterior tolerance for embedded elements.

If an embedded node is located inside the specified tolerance zone, the node is constrained to the host elements. The position of this node will be adjusted to move the node precisely onto the host elements. If an embedded node is located outside the specified tolerance zone, an error message will be issued.

EMBEDDED ELEMENT, EXTERIOR TOLERANCE=tolerance

EMBEDDED ELEMENT,
ABSOLUTE EXTERIOR TOLERANCE=tolerance

Interaction module: Create Constraint: Embedded region: Fractional exterior tolerance or Absolute exterior tolerance

If an embedded node lies close to an element edge or an element face within a host element, it is computationally efficient to make a small adjustment to the position of the embedded node so that the node will lie precisely on the edge or face of the host element. A small tolerance, below which the weight factors of the nodes on a host element associated with an embedded node will be zeroed out, is defined. The small weight factors will be redistributed to the other nodes on the host element in proportion to their initial weights, and the position of the embedded node will be adjusted based on the new weight factors. This adjustment is performed only at the start of the analysis and does not create any strain in the model. It is most useful for making small adjustments to make the embedded nodes lie on the edge or face of a host element. If a large nondefault value of the roundoff tolerance is used to make significant adjustments to the positions of the embedded nodes, you should carefully review the mesh obtained after adjusting.

EMBEDDED ELEMENT, ROUNDOFF TOLERANCE=tolerance

Interaction module: Create Constraint: Embedded region: Weight factor roundoff tolerance

 If an embedded node is also tied by multi-point, equation, kinematic coupling, surface-based tie, or rigid body constraints, an overconstraint is introduced and an error message will be issued. If a boundary condition is applied to an embedded node, the embedded element definition always takes precedence. The boundary condition will be neglected, and a warning message will be issued.

The faces of the embedded elements are not considered part of the all-inclusive surface defined automatically for interactions modeled with general contact, regardless of whether the elements are specified as fully or partially embedded. In addition, any surface definitions based on these elements must have the face identifier specified explicitly (see Element-Based Surface Definition).

The following limitations exist for the embedded element technique:

• Elements with rotational degrees of freedom (except axisymmetric elements with twist) cannot be used as host elements.

• Rotational, temperature, acoustic pressure, and electrical potential degrees of freedom at an embedded node are not constrained.

• Host elements cannot be embedded themselves.

• The material defined for the host element is not replaced by the material defined for the embedded element at the same location of the integration point.

• Additional mass and stiffness due to the embedded elements are added to the model.

• If modified tetrahedron elements are used as host elements, only the corner nodes are used to constrain the appropriate embedded nodes.

Consider the example in Figure 2. Elements 3 (truss) and 4 (membrane) lie embedded in elements 1 and 2. Element 1 is formed by nodes a, b, c, d, e, f, g, and h; element 2 is formed by nodes e, f, g, h, i, j, k, and l; element 3 is formed by nodes A and B; and element 4 is formed by nodes C, D, E, and F. If the host element set includes elements 1 and 2 and the embedded element sets contain elements 3 and 4, respectively, Abaqus will attempt to find if there are any embedded nodes (A, B, C, D, E, and F) lying within host elements 1 or 2. If node A is found to be lying close to the a-b-f-e face of element 1, all the degrees of freedom at node A are constrained to nodes a, b, f, and e, with appropriate weight factors being determined based on the geometric location of node A in element 1. Similarly, if node B is found to be lying inside element 1 and node E is found to be lying close to the g–k edge of element 2, respectively, all the degrees of freedom at node B are constrained to nodes a, b, c, d, e, f, g, and h, and all the degrees of freedom at node E are constrained to nodes g and k, with appropriate weight factors being determined based on the geometric location of node B in element 1 and the geometric location of node E on the g–k edge of element 2, respectively.

Figure 2. Elements lie embedded in host elements.

You should make sure that all the nodes on the desired embedded elements are properly constrained to nodes on the host elements. This can be verified by performing a data check analysis (see Abaqus/Standard and Abaqus/Explicit Execution). For each embedded node a list of nodes that are used to constrain this node and the associated weight factors are output to the data file during the data check analysis. An error message is issued if an embedded node is not constrained and full embedment is used.

HEADING
…
NODE
Data line to define the nodal coordinates
ELEMENT, TYPE=C3D8, ELSET=SOLID3D
Data line to define the solid elements
ELEMENT, TYPE=T3D2, ELSET=TRUSS
Data line to define the truss elements
ELEMENT, TYPE=M3D4, ELSET=MEMB
Data line to define the membrane elements
EMBEDDED ELEMENT, EXTERIOR TOLERANCE=tolerance, HOST ELSET=SOLID3D
TRUSS, MEMB
STEP
STATIC (or any other allowable procedure)
Data line to define step time and control incrementation
…
END STEP