Abaqus has an extensive element library to provide a powerful set of tools for solving many different problems.

Characterizing elements

Five aspects of an element characterize element’s behavior:

• Family
• Degrees of freedom (directly related to the element family)
• Number of nodes
• Formulation
• Integration

Each element in Abaqus has a unique name, such as T2D2, S4R, C3D8I, or C3D8R. The element name identifies each of the five aspects of an element.

Family

Figure 1 shows the element families that are used most commonly in a stress analysis. One of the major distinctions between different element families is the geometry type that each family assumes.

Naming Convention

Each element family is identified by unique naming convention. Please find below naming convention for Continuum elements.

Degrees Of Freedom (DOF)

The degrees of freedom are the fundamental variables calculated during the analysis. For a stress/displacement simulation the degrees of freedom are the translations and, for shell, pipe, and beam elements, the rotations at each node. For a heat transfer simulation the degrees of freedom are the temperatures at each node; for a coupled thermal-stress analysis temperature degrees of freedom exist in addition to displacement degrees of freedom at each node. The degrees of freedom are always referred to as follows:

Here the x-, y-, and z-directions coincide with the global X-, Y-, and Z-directions, respectively.

A maximum of 20 temperature values (degrees of freedom 11 through 30) can be defined for shell or beam elements in Abaqus/Standard.

Number of nodes and order of interpolation

Displacements or other degrees of freedom are calculated at the nodes of the element. At any other point in the element, the displacements are obtained by interpolating from the nodal displacements. Usually the interpolation order is determined by the number of nodes used in the element.

• Elements that have nodes only at their corners, such as the 8-node brick shown in Figure 2 (a), use linear interpolation in each direction and are often called linear elements or first-order elements.
• In Abaqus/Standard elements with midside nodes, such as the 20-node brick shown in Figure 2 (b), use quadratic interpolation and are often called quadratic elements or second-order elements.
• Modified triangular or tetrahedral elements with midside nodes, such as the 10-node tetrahedron shown in Figure 2 (c), use a modified second-order interpolation and are often called modified or modified second-order elements.

Typically, the number of nodes in an element is clearly identified in its name. The 8-node brick element is called C3D8, and the 4-node shell element is called S4R.

Formulation

An element's formulation refers to the mathematical theory used to define the element's behavior. In the Lagrangian, or material, description of behavior the element deforms with the material. In the alternative Eulerian, or spatial, description elements are fixed in space as the material flows through them. Eulerian methods are used commonly in fluid mechanics simulations. Abaqus/Standard uses Eulerian elements to model convective heat transfer. Abaqus/Explicit also offers multimaterial Eulerian elements for use in stress/displacement analyses.

Some Abaqus/Standard element families have a standard formulation as well as some alternative formulations. Elements with alternative formulations are identified by an additional character at the end of the element name. For example, the continuum, beam, and truss element families include members with a hybrid formulation (to deal with incompressible or inextensible behavior); these elements are identified by the letter H at the end of the name (C3D8H or B31H).

Integration

Abaqus uses numerical techniques to integrate various quantities over the volume of each element, thus allowing complete generality in material behavior. Using Gaussian quadrature for most elements, Abaqus evaluates the material response at each integration point in each element. Some continuum elements in Abaqus can use full or reduced integration, a choice that can have a significant effect on the accuracy of the element for a given problem.

Abaqus uses the letter R at the end of the element name to label reduced-integration elements. For example, CAX4R is the 4-node, reduced-integration, axisymmetric, solid element.

👉 Please check the below video to understand Element Selection in the 3DEXPERIENCE Platform.

https://youtu.be/xtCsyBgyRUY

Edu ​​​​​​​

👉 In the next blog, we will get into more details of Solid (continuum) elements. Please stay tuned… ⏳