<!-- source-page: 271 -->

# Constraints

In Abaqus/Standard nodes on a rigid body, excluding the rigid body reference node, cannot be used in a multi-point constraint or linear constraint equation definition.

In Abaqus/Explicit a multi-point constraint or linear constraint equation can be defined for any node on a rigid body, including the reference node.

# Connector elements

Connector elements can be used at any node of a rigid body, including the reference node, to define a connection between rigid bodies, between a rigid body and a deformable body, or from a rigid body to ground. Connector elements are convenient for providing multiple points of attachment on rigid bodies; modeling complex nonlinear kinematic constraints; specifying zero or nonzero boundary conditions at a point on a rigid body that is not the rigid body reference node; applying force actuation; and modeling discrete interactions, such as spring, dashpot, node-to-node contact, friction, locking mechanisms, and failure joints. Unlike multi-point constraints or linear constraint equations, connector elements retain degrees of freedom in the connection, thereby allowing output of information related to the connection (such as constraint forces and moments, relative displacements, velocities, accelerations, etc.). See “Connector elements,” Section 31.1.2, for a detailed description of connector elements.

# Planar rigid body

A rigid body with a planar geometry has three active degrees of freedom: 1, 2, and $6 \ : ( u _ { x } , \ : u _ { y }$ , and ). Here, the x- and y-directions coincide with the global X- and Y-directions, respectively. If a nodal transformation is defined at the rigid body reference node, the x- and y-directions coincide with the userdefined local directions. The coordinate transformation defined at the reference node must be consistent with the geometry; the local directions must remain in the global X–Y plane. All nodes and elements that are part of a planar rigid body should lie in the global X–Y plane.

Planar rigid bodies should be connected only to planar deformable elements. To model the connection of a rigid component with a planar geometry to three-dimensional deformable elements, model the planar rigid component as a three-dimensional rigid body consisting of the appropriate three-dimensional elements.

# Axisymmetric rigid body

A rigid body with an axisymmetric geometry has three active degrees of freedom in Abaqus: 1, 2, and $6 \left( u _ { r } , u _ { z } , \phi \right)$ . Classical axisymmetric theory admits only one rigid body mode, which is displacement in the z-direction. To maximize the flexibility of using rigid bodies for axisymmetric analysis, Abaqus allows for three active degrees of freedom, although only the axial displacement is a rigid body mode.

The r- and z-directions coincide with the global X- and Y-directions, respectively. If a nodal transformation is defined at the rigid body reference node, the r- and z-directions coincide with the user-defined local directions. The coordinate transformation defined at the reference node must be consistent with the geometry; the local directions must remain in the global X–Y plane. All nodes and elements that are part of an axisymmetric rigid body should lie in the global X–Y plane.

<!-- source-page: 272 -->

Translation in the r-direction is associated with a radial mode, and rotation in the r–z plane is associated with a rotary mode (see Figure 2.4.1–2). For an axisymmetric rigid body in Abaqus each of these modes develop no hoop stress, but mass and inertia computed for these degrees of freedom represent the modal mass associated with their modal motion. The mass properties for an axisymmetric rigid body are, therefore, calculated based on the initial configuration assuming the following:

• Point masses defined on nodes of the rigid body (see “Point masses,” Section 30.1.1) are assumed to account for the entire mass around the circumference of the body.   
• Mass contributions from axisymmetric elements assigned to the rigid body include the integrated value around the circumference.   
• The center of mass of the rigid body is located at the center of mass of the circumferential slice, as shown in Figure 2.4.1–2.

If the rigid body reference node is positioned at the center of mass, the reference node for an axisymmetric rigid body will, thus, be repositioned at the center of mass of the circumferential slice.

These assumptions are consistent with the manner in which Abaqus handles other axisymmetric features but are noted here because of the deviation from classical rigid body theory.

Axisymmetric rigid bodies should be connected only to axisymmetric deformable elements. To model the connection of a rigid component with an axisymmetric geometry to three-dimensional deformable elements, model the axisymmetric rigid component as a three-dimensional rigid body consisting of the appropriate three-dimensional elements.

# Three-dimensional rigid body

A rigid body with a three-dimensional geometry has six active degrees of freedom: 1, 2, 3, 4, 5, and $6 \left( u _ { x } , u _ { y } , u _ { z } , \phi _ { x } , \phi _ { y } , \phi _ { z } \right)$ . Here, the x-, y-, and z-directions coincide with the global X-, Y- and Zdirections, respectively. If a nodal transformation is defined at the rigid body reference node, the x-, y-, and z-directions coincide with the user-defined local directions.

In general, three-dimensional rigid bodies will possess a full, nonisotropic inertia tensor and can behave in a nonintuitive manner when they are spun about an axis that is not one of the principal inertia axes. Classical phenomena of rigid body dynamics (e.g., precession, gyroscopic moments, etc.) can be simulated using three-dimensional rigid bodies in Abaqus.

In most cases three-dimensional rigid bodies should be connected only to three-dimensional deformable elements. If it is physically relevant, a three-dimensional rigid body can be connected to two-dimensional plane stress, plane strain, or axisymmetric elements; however, you should always constrain the z-displacement, x-axis rotation, and y-axis rotation of the rigid body. The above procedure is useful when incorporating a two-dimensional plane strain approximation in one region of a model and a three-dimensional discretization in another. Rigid bodies can be used to constrain the two finite element geometries at their interface as shown in Figure 2.4.1–3. A unique rigid body should be used at each node in the plane along the interface to handle the constraint properly.

# Defining loads on rigid bodies

Loads on a rigid body are assembled from contributions of all of the loads on nodes and elements that are part of the rigid body. Loads are defined on nodes and elements that are part of a rigid body in the

<!-- source-page: 273 -->

![](images/page-273_348d76504c1048ff8f6fde015746efb66384444d3d18c73911ca7121304f8d45.jpg)  
Figure 2.4.1–2 Axisymmetric rigid body modes.

same manner that they are specified if the nodes and elements are not part of a rigid body. Contributions include:

• applied concentrated forces on pin nodes, tie nodes, and the rigid body reference node;   
• applied concentrated moments on tie nodes and the rigid body reference node; and   
• applied distributed loads on all elements and surfaces that are part of the rigid body.

<!-- source-page: 274 -->

![](images/page-274_214403c72902aa0b6b62ad79f35b4cdec576e6be7fe5635964e192ab6343d1cf.jpg)

<details>
<summary>text_image</summary>

Y
rigid body
3D mesh
2D mesh
rigid body
X
</details>

Figure 2.4.1–3 Rigid body nodes used to connect a two-dimensional and three-dimensional mesh.

Unless the point of action is through the rigid body center of mass, each of these loads will create both a force at and a torque about the center of mass, which will tend to rotate an unconstrained rigid body. If a nodal transformation is defined at any rigid body nodes, concentrated loads defined at these nodes are interpreted in the local system. The local system defined by the nodal transformation does not rotate with the rigid body.

Concentrated moments defined on rigid body pin nodes do not contribute load to the rigid body but are rather associated with the independent rotation of that node. Independent rotation of a pin node exists only if it is connected to a deformable element with rotational degrees of freedom or a rotary inertia element. Follower forces (see “Specifying concentrated follower forces” in “Concentrated loads,” Section 34.4.2) can be defined at pin nodes if the independent rotation exists. However, the results may be nonintuitive since the direction of the force is determined by the independent rotation even though the follower force acts on the rigid body.

# Rigid bodies with temperature degrees of freedom

Only rigid bodies that contain coupled temperature-displacement elements have temperature degrees of freedom. If it is reasonable to assume that a rigid body used in a fully coupled temperature-displacement analysis has a uniform temperature, you can define the rigid body as isothermal. A transient heat transfer process involving an isothermal rigid body assumes that the internal resistance of the body to heat is negligible in comparison with the external resistance. Thus, the body temperature can be a function of time but cannot be a function of position. The temperature degree of freedom that is created at the rigid body reference node describes the temperature of the body.

Thermal interactions for rigid bodies with analytical rigid surfaces are available only in Abaqus/Explicit and are activated by specifying that the rigid body is isothermal.

<!-- source-page: 275 -->

By default, rigid bodies are not considered isothermal and all nodes on a rigid body connected to coupled temperature-displacement elements will have independent temperature degrees of freedom. The fact that the nodes are part of a rigid body does not affect the ability of the coupled elements to conduct heat within the rigid body. However, the mechanical response will be rigid.

The lumped heat capacitance associated with the rigid body reference node of an isothermal body is calculated automatically if the rigid body is composed of coupled temperature-displacement elements for which a specific heat and a density property are defined. Otherwise, you should specify a point heat capacitance for the rigid body (see “Point capacitance,” Section 30.4.1). An error message will be issued in Abaqus/Explicit if no heat capacitance is associated with an isothermal rigid body for which temperature is not prescribed at the reference node.

• The capacitance of each coupled temperature-displacement element that is part of the rigid body contributes to the isothermal rigid body’s capacitance. For an axisymmetric isothermal rigid body, capacitance contributions from axisymmetric elements assigned to the rigid body include the integrated value around the circumference.   
• HEATCAP elements that are connected to any node that is part of a rigid body or the rigid body reference node contribute to the isothermal rigid body’s capacitance. For an axisymmetric isothermal rigid body the point capacitances defined on nodes of the rigid body are assumed to account for the capacitance integrated around the circumference of the body.

Thermal loads acting on the reference node of an isothermal body are assembled from contributions of all the thermal loads on nodes and elements that are part of the rigid body. Heat transfer between a deformable body and an isothermal rigid body can occur during contact, as well as when the bodies are not in contact if gap conductance and gap radiation are defined (see “Thermal contact properties,” Section 37.2.1). Heat transfer between two isothermal rigid bodies can occur only via gap conduction and gap radiation.

Input File Usage: \*RIGID BODY, ISOTHERMAL=YES

Abaqus/CAE Usage: Interaction module: Create Constraint: Rigid body: toggle on Constrain selected regions to be isothermal

# Modeling contact with a rigid body

Contact with a rigid body is modeled by specifying a contact interaction formed with a rigid surface and with a surface defined on another body (see “Defining contact pairs in Abaqus/Standard,” Section 36.3.1; “Defining general contact interactions in Abaqus/Explicit,” Section 36.4.1; or “Defining contact pairs in Abaqus/Explicit,” Section 36.5.1). A rigid surface can be formed by nodes, element faces, or an analytical surface (see “Node-based surface definition,” Section 2.3.3; “Element-based surface definition,” Section 2.3.2; and “Analytical rigid surface definition,” Section 2.3.4).

Contact modeling can be a primary factor when choosing the appropriate rigid body geometry. Contact interactions should be formed with surfaces of like geometry. For example, a planar rigid body should be used to model contact either with deformable surfaces formed by two-dimensional plane stress or plane strain elements or via node-based surfaces with two-dimensional beam, pipe, or truss elements. Similarly, an axisymmetric rigid body should be used to model contact with surfaces formed by

<!-- source-page: 276 -->

axisymmetric elements, and a three-dimensional rigid body should be used to model contact either with surfaces formed by three-dimensional element faces or via node-based surfaces with three-dimensional beam, pipe, or truss elements.

A rigid body must contain only two-dimensional or only three-dimensional elements. Nodes cannot be shared between two rigid bodies. Contact between two analytical rigid surfaces or between an analytical rigid surface and itself cannot be modeled.

# Limitations in Abaqus/Standard

Contact between rigid bodies is allowed if the slave surface belongs to an elastic body that has been declared as rigid. In this case softened contact should be prescribed to avoid possible overconstraints.

Contact between two rigid surfaces defined using rigid elements is not allowed.

Rigid beams and trusses cannot be included in a contact pair definition because surfaces from beams and trusses can be node-based surfaces only. A node-based surface must be a slave surface, and elements that are part of a rigid body should be part of the master surface in a contact pair.

# Limitations in Abaqus/Explicit

Contact between two rigid surfaces can be modeled in Abaqus/Explicit only if the penalty contact pair algorithm or the general contact algorithm is used; kinematic contact pairs cannot be used for rigidto-rigid contact. Therefore, when converting two deformable regions of a model to two distinct rigid bodies for the purpose of model development, any contact interaction definitions between these rigid bodies must use penalty contact pairs or general contact.

For rigid-to-rigid contact involving analytical rigid surfaces, at least one of the rigid surfaces must be formed by element faces since contact between two analytical rigid surfaces cannot be modeled in Abaqus.

The penalty contact pair algorithm, which introduces numerical softening to the contact enforcement through the use of penalty springs, or the general contact algorithm must be used for all contact interactions involving a rigid body if an equation constraint, a multi-point constraint, a tie constraint, or a connector element is defined for a node on the rigid body.

Rigid beams and trusses cannot be included in a kinematic contact pair definition because surfaces from beams and trusses can be node-based surfaces only. A node-based surface must be a slave surface, and elements that are part of a rigid body must be part of the master surface in a kinematic contact pair.

When a rigid surface acts as a slave surface in a penalty contact pair or in general contact, initial penetrations of the rigid slave nodes into the master surface will not be corrected with strain-free corrections (see “Adjusting initial surface positions and specifying initial clearances for contact pairs in Abaqus/Explicit,” Section 36.5.4, and “Controlling initial contact status for general contact in Abaqus/Explicit,” Section 36.4.4). For contact pairs any initial penetrations of this type may cause artificially large contact forces in the initial increments. For general contact these initial penetrations are stored as contact offsets.

<!-- source-page: 277 -->

# Using rigid bodies in geometrically linear Abaqus/Standard analysis

If rigid bodies are used in a geometrically linear Abaqus/Standard analysis (see “General and linear perturbation procedures,” Section 6.1.3), the rigid body constraints are linearized. Consequently, except for analytical rigid surfaces, the distance between any two nodes belonging to the rigid body may not remain constant during the analysis if the magnitudes of the rotations are not small.

<!-- source-page: 278 -->

<!-- source-page: 279 -->

# 2.5 Integrated output section definition

• “Integrated output section definition,” Section 2.5.1

<!-- source-page: 280 -->
