<!-- source-page: 531 -->

# 30.2.1 ROTARY INERTIA

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

# References

• “Rotary inertia element library,” Section 30.2.2   
• \*ROTARY INERTIA   
• “Defining point mass and rotary inertia,” Section 33.3 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

# Overview

Rotary inertia elements:

• allow rotary inertia to be included at a node;   
• are associated with the three rotational degrees of freedom at a node; and   
• can be paired with a MASS element (“Point masses,” Section 30.1.1) to define the mass and inertia properties of a rigid body directly (“Rigid body definition,” Section 2.4.1).

# Defining the rotary inertia

The ROTARYI element allows rotary inertia to be included at a node. The node is assumed to be the center of mass of the body so that only second moments of inertia are required. If the node is part of a rigid body, the offset between the node and the center of mass of the rigid body is accounted for. All six components of the rotary inertia tensor— $- I _ { 1 1 } , I _ { 2 2 } , I _ { 3 3 } , I _ { 1 2 } , I _ { 1 3 }$ , and $I _ { 2 3 }$ —about the global coordinate system are defined as follows:

$$
I _ {1 1} = \int_ {V} \rho \left((x _ {2}) ^ {2} + (x _ {3}) ^ {2}\right) d V
$$

$$
I _ {2 2} = \int_ {V} \rho \big ((x _ {3}) ^ {2} + (x _ {1}) ^ {2} \big) d V
$$

$$
I _ {3 3} = \int_ {V} \rho \bigl ((x _ {1}) ^ {2} + (x _ {2}) ^ {2} \bigr) d V
$$

$$
I _ {1 2} = - \int_ {V} \rho (x _ {1} x _ {2}) d V
$$

$$
I _ {1 3} = - \int_ {V} \rho (x _ {1} x _ {3}) d V
$$

$$
I _ {2 3} = - \int_ {V} \rho (x _ {2} x _ {3}) d V.
$$

The rotary inertia tensor must be positive semi-definite.

<!-- source-page: 532 -->

You specify the moments of inertia, which should be given in units of $\mathrm { { M L } } ^ { 2 }$ . You must associate these moments of inertia with a region of your model.

Optionally, you can refer to a local orientation (“Orientations,” Section 2.2.5) that defines the directions of the local axes for which the rotary inertia values are being given. If you do not specify a local orientation and the rotary inertia element is defined within a part or a part instance (see “Defining an assembly,” Section 2.10.1), the components of the inertia tensor must be given with respect to the local part axes. If you do not specify a local orientation and the rotary inertia element is not defined within a part or a part instance, the components of the inertia tensor must be given with respect to the global axes.

Input File Usage: \*ROTARY INERTIA, ELSET=name, ORIENTATION=name $I _ { 1 1 } , I _ { 2 2 } , I _ { 3 3 } , I _ { 1 2 } , I _ { 1 3 } , I _ { 2 3 }$

where the ELSET parameter refers to a set of ROTARYI elements.

Abaqus/CAE Usage: Property or Interaction module: Special→Inertia→Create: Point mass/inertia: select point: Magnitude: I11: $I _ { 1 1 }$ , I22: $I _ { 2 2 }$ , I33: $I _ { 3 3 } { \mathrm { : } }$ ; if necessary, toggle on Specify off-diagonal terms: I12: $I _ { 1 2 }$ , I13: $I _ { 1 3 }$ , I23: $I _ { 2 3 } ;$ CSYS: Edit

# Defining damping for ROTARYI elements

In Abaqus/Standard you can define mass proportional damping for direct-integration dynamic analysis or composite damping for modal dynamic analysis. Although both damping definitions can be specified for a set of ROTARYI elements, only the damping that is relevant to the particular dynamic analysis procedure will be used.

In Abaqus/Explicit mass proportional damping can be defined for ROTARYI elements.

# Dynamics

You can define inertia proportional damping for ROTARYI elements in direct-integration dynamic analysis or explicit dynamic analysis. See “Material damping,” Section 26.1.1, for details.

Input File Usage: \*ROTARY INERTIA, ALPH $\scriptstyle \mathbf { A } = \alpha _ { R }$

Abaqus/CAE Usage: Property or Interaction module: Special→Inertia→Create: Point mass/inertia: select point: Damping: Alpha: $\alpha _ { R }$

# Modal dynamics

You can define the fraction of critical damping to be used with the ROTARYI elements when calculating composite damping factors for the modes when used in modal dynamic analysis. See “Material damping,” Section 26.1.1, for details.

Input File Usage: \*ROTARY INERTIA, COMPOSITE=

Abaqus/CAE Usage: Property or Interaction module: Special→Inertia→Create: Point mass/inertia: select point: Damping: Composite: $\xi _ { \alpha }$

<!-- source-page: 533 -->

# Speeding up convergence in three-dimensional implicit analyses

In geometrically nonlinear analysis in Abaqus/Standard, rigid body rotary inertia contributes some unsymmetric terms to the system matrix when the motion is in three dimensions and the rotary inertia is not the same about all three axes. Therefore, in cases when the rotary inertia effects are significant, the solution may converge faster if you use the unsymmetric matrix storage and solution scheme for the step (“Defining an analysis,” Section 6.1.2).

<!-- source-page: 534 -->

<!-- source-page: 535 -->

# 30.2.2 ROTARY INERTIA ELEMENT LIBRARY

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

# References

• “Rotary inertia,” Section 30.2.1   
• \*ROTARY INERTIA

# Overview

This section provides a reference to the rotary inertia elements available in Abaqus/Standard and Abaqus/Explicit.

# Element type

ROTARYI Rotary inertia at a point

Active degrees of freedom

4, 5, 6

Additional solution variables

None.

# Nodal coordinates required

X, Y, Z

# Element property definition

Input File Usage: \*ROTARY INERTIA

Abaqus/CAE Usage: Property or Interaction module: Special→Inertia→Create: Point mass/inertia: select point: Magnitude: Rotary Inertia

# Element-based loading

# Distributed loads

Distributed loads are specified as described in “Distributed loads,” Section 34.4.3.

<!-- source-page: 536 -->

<table><tr><td>Load ID(*DLOAD)</td><td>Abaqus/CAE Load/Interaction</td><td>Units</td><td>Description</td></tr><tr><td> $\text{ROTA}^{(S)}$ </td><td>Not supported</td><td> $T^{-2}$ </td><td>Rotary acceleration load (magnitude is input as  $\alpha$ , where  $\alpha$  is the rotary acceleration).</td></tr><tr><td> $\text{ROTDYNF}^{(S)}$ </td><td>Not supported</td><td> $T^{-1}$ </td><td>Rotordynamic load (magnitude is input as  $\omega$ , where  $\omega$  is the angular velocity).</td></tr></table>

Element output

ELKE Element kinetic energy (available only from Abaqus/Standard).

Nodes associated with the element

1 node.

<!-- source-page: 537 -->

# 30.3 Rigid elements

• “Rigid elements,” Section 30.3.1   
• “Rigid element library,” Section 30.3.2

<!-- source-page: 538 -->

<!-- source-page: 539 -->

# 30.3.1 RIGID ELEMENTS

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CAE

# References

• “Rigid body definition,” Section 2.4.1   
• “Rigid element library,” Section 30.3.2   
• \*RIGID BODY   
• “Defining rigid body constraints,” Section 15.15.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

# Overview

Rigid elements:

• can be used to define the surfaces of rigid bodies for contact;   
• can be used to define rigid bodies for multibody dynamic simulations;   
• can be attached to deformable elements;   
• can be used to constrain parts of a model;   
• are used to apply Abaqus/Aqua loads to rigid structures; and   
• are associated with a given rigid body and share a common node known as the rigid body reference node.

# Choosing an appropriate element

Use R2D2 elements in plane strain or plane stress analysis, RAX2 elements in axisymmetric planar geometries, and R3D3 and R3D4 elements in three-dimensional analysis.

RB2D2 and RB3D2 elements are often used in Abaqus/Standard to model offshore structures that will transmit Abaqus/Aqua loads but will not deform. They can also be used as rigid links between nodes on deformable bodies.

# Naming convention

Rigid elements in Abaqus are named as follows:

<!-- source-page: 540 -->

![](images/page-540_ed1489d87c0fa7f2aac1d7e8d6ef36fbf62cfde9fbdd1219cfc97bb130e344d2.jpg)

<details>
<summary>text_image</summary>

R B 3D 2
number of nodes
two-dimensional (2D),
three-dimensional (3D),
or axisymmetric (AX)
beam (optional)
rigid element
</details>

For example, R2D2 is a two-dimensional, 2-node, rigid element.

# Element normal definition

For all rigid elements the face on the side of the element with the positive outward normal is referred to as SPOS. The face on the opposite side is referred to as SNEG. The positive normal direction for each element is defined below.

R2D2, RAX2, RB2D2, R3D3, and R3D4 rigid elements can be used in Abaqus/Standard to define master surfaces for contact applications. The direction of the master surface’s outward normal is critical for proper detection of contact. See “Defining contact pairs in Abaqus/Standard,” Section 36.3.1, for a more detailed discussion of contact surface definitions.

# Two-dimensional rigid elements

The positive outward normal direction, , is defined by a 90° counterclockwise rotation from the direction going from node 1 to node 2 of the element. See Figure 30.3.1–1.

![](images/page-540_e69a23ed5fe404ae0a437a1f07ddfe1ef154fd39d8c568584ed3405d3151a277.jpg)

<details>
<summary>text_image</summary>

Y or z
X or r
n
face SPOS
2
face SNEG
1
</details>

Figure 30.3.1–1 Positive normal for two-dimensional rigid elements.

# Three-dimensional rigid elements

The positive normal for R3D3 and R3D4 elements is given by the right-hand rule going around the nodes of the element in the order that they are given in the element’s connectivity. See Figure 30.3.1–2.

RB3D2 elements do not have a unique normal definition.
