<!-- source-page: 31 -->

Contact modeling if substructures are present 37.3.9

Contact modeling if asymmetric-axisymmetric elements are present 37.3.10

# Defining general contact in Abaqus/Explicit

Defining general contact interactions in Abaqus/Explicit 37.4.1

Assigning surface properties for general contact in Abaqus/Explicit 37.4.2

Assigning contact properties for general contact in Abaqus/Explicit 37.4.3

Controlling initial contact status for general contact in Abaqus/Explicit 37.4.4

Contact controls for general contact in Abaqus/Explicit 37.4.5

# Defining contact pairs in Abaqus/Explicit

Defining contact pairs in Abaqus/Explicit 37.5.1

Assigning surface properties for contact pairs in Abaqus/Explicit 37.5.2

Assigning contact properties for contact pairs in Abaqus/Explicit 37.5.3

Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit 37.5.4

Contact controls for contact pairs in Abaqus/Explicit 37.5.5

# 38. Contact Property Models

# Mechanical contact properties

Mechanical contact properties: overview 38.1.1

Contact pressure-overclosure relationships 38.1.2

Contact damping 38.1.3

Contact blockage 38.1.4

Frictional behavior 38.1.5

User-defined interfacial constitutive behavior 38.1.6

Pressure penetration loading 38.1.7

Interaction of debonded surfaces 38.1.8

Breakable bonds 38.1.9

Surface-based cohesive behavior 38.1.10

# Thermal contact properties

Thermal contact properties 38.2.1

# Electrical contact properties

Electrical contact properties 38.3.1

# Pore fluid contact properties

Pore fluid contact properties 38.4.1

# 39. Contact Formulations and Numerical Methods

# Contact formulations and numerical methods in Abaqus/Standard

Contact formulations in Abaqus/Standard 39.1.1

<!-- source-page: 32 -->

Contact constraint enforcement methods in Abaqus/Standard 39.1.2

Smoothing contact surfaces in Abaqus/Standard 39.1.3

# Contact formulations and numerical methods in Abaqus/Explicit

Contact formulation for general contact in Abaqus/Explicit 39.2.1

Contact formulations for contact pairs in Abaqus/Explicit 39.2.2

Contact constraint enforcement methods in Abaqus/Explicit 39.2.3

# 40. Contact Difficulties and Diagnostics

# Resolving contact difficulties in Abaqus/Standard

Contact diagnostics in an Abaqus/Standard analysis 40.1.1

Common difficulties associated with contact modeling in Abaqus/Standard 40.1.2

# Resolving contact difficulties in Abaqus/Explicit

Contact diagnostics in an Abaqus/Explicit analysis 40.2.1

Common difficulties associated with contact modeling using contact pairs in Abaqus/Explicit 40.2.2

# 41. Contact Elements in Abaqus/Standard

# Contact modeling with elements

Contact modeling with elements 41.1.1

# Gap contact elements

Gap contact elements 41.2.1

Gap element library 41.2.2

# Tube-to-tube contact elements

Tube-to-tube contact elements 41.3.1

Tube-to-tube contact element library 41.3.2

# Slide line contact elements

Slide line contact elements 41.4.1

Axisymmetric slide line element library 41.4.2

# Rigid surface contact elements

Rigid surface contact elements 41.5.1

Axisymmetric rigid surface contact element library 41.5.2

# 42. Defining Cavity Radiation in Abaqus/Standard

# Defining cavity radiation

Cavity radiation 42.1.1

<!-- source-page: 33 -->

# Part VI: Elements

• Chapter 27, “Elements: Introduction”   
• Chapter 28, “Continuum Elements”   
• Chapter 29, “Structural Elements”   
• Chapter 30, “Inertial, Rigid, and Capacitance Elements”   
• Chapter 31, “Connector Elements”   
• Chapter 32, “Special-Purpose Elements”   
• Chapter 33, “Particle Elements”

<!-- source-page: 34 -->

<!-- source-page: 35 -->

# 27. Elements: Introduction

Introduction

27.1

<!-- source-page: 36 -->

<!-- source-page: 37 -->

# 27.1 Introduction

• “Element library: overview,” Section 27.1.1   
• “Choosing the element’s dimensionality,” Section 27.1.2   
• “Choosing the appropriate element for an analysis type,” Section 27.1.3   
• “Section controls,” Section 27.1.4

<!-- source-page: 38 -->

<!-- source-page: 39 -->

# 27.1.1 ELEMENT LIBRARY: OVERVIEW

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 its 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. For details on defining elements, see “Element definition,” Section 2.2.1.

# Family

Figure 27.1.1–1 shows the element families that are used most commonly in a stress analysis; in addition, continuum (fluid) elements are used in a fluid analysis. One of the major distinctions between different element families is the geometry type that each family assumes.   
![](images/page-039_a8c65de245e08a8c30e8ba0a601ab9fe215ec7b5aa4e869cda26fd47cc0fdb1e.jpg)  
Figure 27.1.1–1 Commonly used element families.

The first letter or letters of an element’s name indicate to which family the element belongs. For example, S4R is a shell element, CINPE4 is an infinite element, and C3D8I is a continuum element.

<!-- source-page: 40 -->

# Degrees of freedom

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. Heat transfer analyses and coupled thermal-stress analyses therefore require the use of different elements than does a stress analysis since the degrees of freedom are not the same. See “Conventions,” Section 1.2.2, for a summary of the degrees of freedom available in Abaqus for various element and analysis types.

# 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 27.1.1–2(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 27.1.1–2(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 27.1.1–2(c), use a modified second-order interpolation and are often called modified or modified second-order elements.

![](images/page-040_e6f2db2d83bd2e83e7bfb6225c4376c4a3280f6334352697be3938c4993357ad.jpg)

<details>
<summary>natural_image</summary>

Simple 3D wireframe cube diagram with no text or labels
</details>

(a) Linear element (8-node brick, C3D8)

![](images/page-040_5cbcb5be3312105123f1fd2fdffee32e2b701221f68be2f985bf89d0396e521b.jpg)

<details>
<summary>natural_image</summary>

3D wireframe cube diagram with black dots at vertices and edges, no text or labels present
</details>

(b) Quadratic element (20-node brick, C3D20)

![](images/page-040_739412d37e2119c79fd4219fc596a47cd00c99f901827b84fd9d480763ad4556.jpg)

<details>
<summary>natural_image</summary>

Geometric diagram of a polyhedron with solid and dashed edges (no text or labels)
</details>

(c) Modified second-order element (10-node tetrahedron, C3D10M)   
Figure 27.1.1–2 Linear brick, quadratic brick, and modified tetrahedral 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.

The beam element family uses a slightly different convention: the order of interpolation is identified in the name. Thus, a first-order, three-dimensional beam element is called B31, whereas a second-order, three-dimensional beam element is called B32. A similar convention is used for axisymmetric shell and membrane elements.
