<!-- source-page: 161 -->

Defining global structural damping

You can define the global structural damping factor, , to get

$$
K _ {s} ^ {g} = \mathbf {s} _ {g l o b a l} K.
$$

Global structural damping can be specified for the entire model (default), for the mechanical degree of freedom field (displacements and rotations) only, or for the acoustic field only.

Input File Usage: Use the following option to specify global structural damping:

\*GLOBAL DAMPING, STRUCTURAL=

Abaqus/CAE Usage: Global structural damping is not supported in Abaqus/CAE.

Defining structural modal damping

Structural damping assumes that the damping forces are proportional to the forces caused by stressing of the structure and are opposed to the velocity (see “Structural damping” in “Material damping,” Section 26.1.1, for more information). This form of damping can be used only when the displacement and velocity are exactly 90° out of phase, as in steady-state and random response analyses where the excitation is purely sinusoidal.

Structural damping can be defined as diagonal modal damping for mode-based steady-state dynamic and random response analyses.

Input File Usage: Use the following option to define structural damping by specifying mode numbers:

\*MODAL DAMPING, STRUCTURAL, DEFINITION=MODE NUMBERS

Use the following option to define structural damping by specifying a frequency range:

\*MODAL DAMPING, STRUCTURAL, DEFINITION=FREQUENCY RANGE

Abaqus/CAE Usage: Use the following input to define structural damping by specifying mode numbers:

Step module: Create Step: Linear perturbation: any valid step

type: Damping: Specify damping over ranges of: Modes,

Structural: Use structural damping data

Use the following input to define structural damping by specifying frequency ranges:

Step module: Create Step: Linear perturbation: any valid step

type: Damping: Specify damping over ranges of: Frequencies,

Structural: Use structural damping data

<!-- source-page: 162 -->

# Controlling the sources of structural damping

The material/element and global structural damping sources can be controlled at the step level; controls are not available for modal damping. If both the material/element and global structural damping matrices are supplied, both will be combined unless you request that only the element or global damping factor be used. The combined structural damping matrix is

$$
K _ {s} = K _ {s} ^ {m} + K _ {s} ^ {g}.
$$

Input File Usage: Use the following option to activate only the material/element structural damping matrix:

\*DAMPING CONTROLS, STRUCTURAL=ELEMENT

Use the following option to activate only the global structural damping matrix:

\*DAMPING CONTROLS, STRUCTURAL=FACTOR

Use the following option to activate the combined material/element and global structural damping matrix:

\*DAMPING CONTROLS, STRUCTURAL=COMBINED

Abaqus/CAE Usage: Damping controls are not supported in Abaqus/CAE.

# Excluding structural damping effects

You can choose to exclude the effects of structural damping altogether at the step level.

Input File Usage: Use the following option to exclude structural damping matrix:

\*DAMPING CONTROLS, STRUCTURAL=NONE

Abaqus/CAE Usage: Damping controls are not supported in Abaqus/CAE.

# Defining both viscous and structural damping

The imaginary contribution to the frequency domain dynamics equation, which represents the effect of damping, may include both viscous and structural damping and can be written as

$$
D = \Omega D _ {v i s c o u s} + K _ {s},
$$

where is the forcing frequency.

# Defining composite modal damping

Composite modal damping allows you to define a damping factor for each material or element in the model as a fraction of critical damping. These factors are then combined into a damping factor for each mode as weighted averages of the mass matrix associated with each material or element; when using the SIM architecture, you can also include the weighted averages of the stiffness matrix. Composite modal damping can be defined only by specifying mode numbers; it cannot be defined by specifying a frequency range.

<!-- source-page: 163 -->

Defining composite modal damping for analyses using the traditional architecture

You specify composite modal damping in the material definition for analyses that use the traditional architecture. The damping per eigenmode is calculated as:

$$
\xi_ {\alpha} = \frac {1}{m _ {\alpha}} \phi_ {\alpha} ^ {T} \left(\sum_ {m} \xi_ {m} M _ {m}\right) \phi_ {\alpha},
$$

where $\xi _ { \alpha }$ is the critical damping fraction used in mode $\alpha , \xi _ { m }$ is the critical damping fraction defined for material m, $M _ { m }$ is the mass matrix associated with material $m , \phi _ { \alpha }$ is the eigenvector of mode , and $m _ { \alpha }$ is the generalized mass associated with mode :

$$
m _ {\alpha} = \phi_ {\alpha} ^ {T} M \phi_ {\alpha}.
$$

If you specify composite modal damping, Abaqus calculates the damping coefficients $\xi _ { \alpha }$ in the eigenfrequency extraction step from the damping factors $\xi _ { m }$ that you defined for each material.

Input File Usage: Use both of the following options:

$\ast \mathrm { D A M P I N G } , \mathrm { C O M P O S I T E } { = } \xi _ { m }$

$* { \mathrm { M O D A L ~ D A M P I N G } } , \mathrm { V I S C O U S { = } C O M P O S I T E }$

Abaqus/CAE Usage: Property module: material editor: Mechanical→Damping: Composite: $\xi _ { m }$

Step module: Create Step: Linear perturbation: any valid step $t y p e { \mathrm { : } }$

Damping: Composite modal: Use composite damping data

Defining composite modal damping for analyses using the SIM architecture

You can specify composite modal damping for SIM-based analyses that use the Lanczos eigensolver. Composite modal damping is specified for each element. You can also assign critical damping fractions to both mass and stiffness matrix input. The mass weighted damping per eigenmode is calculated as:

$$
\xi_ {\alpha} ^ {M} = \phi_ {\alpha} ^ {T} M _ {\xi} \phi_ {\alpha} = \phi_ {\alpha} ^ {T} \left(\sum_ {e l e m e n t s} \xi_ {e l e m e n t} ^ {M} m _ {e l e m e n t} + \xi_ {\mathit {\Pi} _ {i n p u t} ^ {m a t r i x}} ^ {M} M _ {\mathit {\Pi} _ {i n p u t} ^ {m a t r i x}}\right) \phi_ {\alpha},
$$

where $\xi _ { \alpha } ^ { M }$ is the mass weighted critical damping fraction used in mode $\alpha , M _ { \xi }$ is a damped portion of the mass matrix, $\xi ^ { M }$ are fractions of critical damping for the element mass matrix and mass matrix input, and $\phi _ { \alpha }$ is the eigenvector of mode .

The stiffness weighted damping per eigenmode is calculated as:

$$
\xi_{\alpha}^{K} = \frac{1}{\omega_{\alpha}^{2}}\phi_{\alpha}^{T}K_{\xi}\phi_{\alpha} = \frac{1}{\omega_{\alpha}^{2}}\phi_{\alpha}^{T}\left(\sum_{\substack{elements}}\xi_{element}^{K}k_{element} + \xi_{\substack{matrix\\ input}}^{K}K_{\substack{matrix\\ input}}\right)\phi_{\alpha},
$$

where $\xi _ { \alpha } ^ { K }$ is the stiffness weighted critical damping fraction used in mode , $K _ { \xi }$ is a damped portion of the stiffness matrix, $\xi ^ { K }$ are fractions of critical damping for the element stiffness and matrix input stiffness, and $\phi _ { \alpha }$ is the eigenvector of mode .

<!-- source-page: 164 -->

<table><tr><td>Input File Usage:</td><td>Use both of the following options to specify composite modal damping:*FREQUENCY, EIGENSOLVER=LANCZOS, SIM*COMPOSITE MODAL DAMPINGUse the following option to specify the fraction of critical damping for all mass matrices included in matrix input:*COMPOSITE MODAL DAMPING, MASS MATRIX INPUTUse the following option to specify the fraction of critical damping for all stiffness matrices included in matrix input:*COMPOSITE MODAL DAMPING, STIFFNESS MATRIX INPUT</td></tr></table>

<table><tr><td>Abaqus/CAE Usage:</td><td>Defining composite modal damping for analyses using the SIM architecture is not supported in Abaqus/CAE.</td></tr></table>

# Defining global damping for acoustic fields

If your model contains acoustic elements, Abaqus applies any specified global damping to both the acoustic fields and the structural fields in the model by default. If desired, you can specify that a global damping definition applies only to the acoustic fields or only to the displacement and rotation fields (not supported in a mode-based steady-state dynamic analysis that uses coupled acoustic-structural modes).

<table><tr><td>Input File Usage:</td><td>Use the following option to apply global damping to all of the displacement, rotation, and acoustic fields in a model:*GLOBAL DAMPING, FIELD=ALL (default)Use the following option to apply global damping only to the acoustic fields in a model:*GLOBAL DAMPING, FIELD=ACOUSTICUse the following option to apply global damping only to the displacement and rotation fields in a model:*GLOBAL DAMPING, FIELD=MECHANICAL</td></tr><tr><td>Abaqus/CAE Usage:</td><td>Global damping is not supported in Abaqus/CAE.</td></tr></table>

# Defining and using both global and modal diagonal damping

Mode-based procedures—such as steady-state dynamics, transient modal dynamic, response spectrum, and random response analyses—can also use a step-dependent, modal damping definition that is specified per eigenmode. When multiple modal damping definitions are used with different damping types, the damping is additive. If the same damping type is specified more than once, the last specification is used. If modal damping is used with global damping, both types of damping will contribute to the damping matrix.

Damping controls have no effect on modal damping. If damping controls are used to exclude certain global damping effects in a step, all modal damping effects are still included in the step. To exclude modal damping, the damping definition must be specifically removed from the step definition.

<!-- source-page: 165 -->

# Controlling damping of low frequency modes

You can include or exclude damping of the low frequency eigenmodes in transient modal analyses. This control is useful for free structures and models with secondary base motions. For details, see “Transient modal dynamic analysis,” Section 6.3.7.

# Acoustic contribution factors in mode-based and subspace-based steady-state dynamic analyses

You can compute acoustic contribution factors for the linear, eigenmode-based, steady-state dynamic procedures. Computation of the acoustic contribution factors makes it possible to answer the following questions:

• Which noise source has the greatest contribution?   
• Which point does the loudest noise come from?   
• Which structural component does the loudest noise come from?   
• Which natural frequency contributes the most to the noise?

By answering these questions you can determine the major noise sources as well as make the necessary changes to your design to reduce the noise levels. The procedure for computing the acoustic contribution factors is based on the modal analysis formulation of acoustic-structural problems with uncoupled modes. It is available in steady-state mode-based and subspace-based dynamic analyses performed using the high-performance SIM architecture. To enable computation of the acoustic contribution factors, the preceding frequency extraction step has to use the uncoupled modes formulation as well as to activate the SIM architecture. Abaqus/Standard supports the computation of the following contribution factors:

• Acoustic modal contribution factors,   
• Acoustic structural modal contribution factors,   
• Acoustic load modal contribution factors,   
• Acoustic load contribution factors,   
• Panel contribution factors, and   
• Grid contribution factors.

The acoustic node set defines a set of the response nodes in the acoustic domain. You can specify up to 20 response nodes in this set. You can also select the acoustic or structural eigenmodes that will be used to compute the modal contribution factors. You specify the lower and upper bounds of the frequency range to apply to the active eigenmodes (see “Selecting the modes and specifying damping” in “Mode-based steady-state dynamic analysis,” Section 6.3.8, and “Selecting the modes on which to project” in “Subspace-based steady-state dynamic analysis,” Section 6.3.9).

The computed contribution factors are saved in the SIM database file. You can retrieve the data as described in “Plug-in utility for visualizing Acoustic Contribution Factors” in the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base.

<!-- source-page: 166 -->

Input File Usage: Use the following option to request computation of the acoustic modal contribution factors:

*ACOUSTIC CONTRIBUTION, NAME=name,
ACOUSTIC NODES=acoustic_nset $f_{min}, f_{max}$

Abaqus/CAE Usage: Specifying acoustic contribution factors is not supported in Abaqus/CAE.

# Specifying acoustic modal contribution factors

Acoustic modal contribution factors show the contribution of each acoustic mode into the total acoustic pressure at the response points. You can also select the acoustic eigenmodes that will be used to compute the contribution factors.

Input File Usage: Use the following option to compute the acoustic modal contribution factors:

```txt
*ACOUSTIC CONTRIBUTION, TYPE=MODAL ACOUSTIC 
```

Abaqus/CAE Usage: Specifying acoustic contribution factors is not supported in Abaqus/CAE.

# Specifying acoustic structural modal contribution factors

Acoustic structural modal contribution factors measure the contribution of each structural mode into the acoustic pressure caused by the structural components. You can also select the structural eigenmodes that will be used to compute the contribution factors.

Input File Usage: Use the following option to compute the acoustic structural modal contribution factors:

```txt
*ACOUSTIC CONTRIBUTION, TYPE=MODAL STRUCTURAL 
```

Abaqus/CAE Usage: Specifying acoustic contribution factors is not supported in Abaqus/CAE.

# Specifying acoustic load modal contribution factors

Acoustic load modal contribution factors define the contribution of each acoustic mode due to the acoustic sources into the acoustic pressure. You can specify the acoustic eigenmodes that are going to be used to compute the contribution factors.

Input File Usage: Use the following option to compute the acoustic load modal contribution factors:

```txt
*ACOUSTIC CONTRIBUTION, TYPE=MODAL LOAD 
```

Abaqus/CAE Usage: Specifying acoustic contribution factors is not supported in Abaqus/CAE.

# Specifying acoustic load contribution factors

Acoustic load contribution factors define the contribution of the acoustic sources into the acoustic pressure.

Input File Usage: Use the following option to compute the acoustic load contribution factors:

```txt
*ACOUSTIC CONTRIBUTION, TYPE=LOAD 
```

<!-- source-page: 167 -->

Abaqus/CAE Usage: Specifying acoustic contribution factors is not supported in Abaqus/CAE.

# Specifying panel contribution factors

Panel contribution factors measure the contribution of the user-defined structural surfaces into the acoustic pressure caused by structural sources.

Optionally, you can specify a set of nodes that defines a structural panel—a set of nodes on the acoustic-structural interface that is considered to be a single noise source. If this node set contains other structural or acoustic nodes that do not belong to the acoustic-structural interface, such nodes are filtered out and are not considered for panel contribution factor computations. If you do not specify a set of nodes on the acoustic-structural interface, all nodes on the interface are used to determine the panel contribution factors.

Input File Usage: Use the following option to compute the panel contribution factor:

```txt
*ACOUSTIC CONTRIBUTION, TYPE=PANEL, STRUCTURAL NODES=structural_nset 
```

Abaqus/CAE Usage: Specifying acoustic contribution factors is not supported in Abaqus/CAE.

# Specifying grid contribution factors

Grid contribution factors measure the contribution of each node on the acoustic-structural interface into the acoustic pressure caused by structural sources.

Optionally, you can specify a set of nodes on the acoustic-structural interface. Each node in this set is considered to be an individual noise source. If this node set contains other structural or acoustic nodes that do not belong to the acoustic-structural interface, such nodes will be filtered out and will not be considered for the grid contribution factor computations. If you do not specify a set of nodes on the acoustic-structural interface, all nodes on the interface are used to determine the grid contribution factors. Due to the large amount of data generated for grid contribution factors, the number of nodes in this node set is limited to 10,000 nodes. If this number is exceeded, the first 10,000 nodes are used.

Input File Usage: Use the following option to compute the grid contribution factor:

```txt
*ACOUSTIC CONTRIBUTION, TYPE=GRID, STRUCTURAL NODES=structural_nset 
```

Abaqus/CAE Usage: Specifying acoustic contribution factors is not supported in Abaqus/CAE.

<!-- source-page: 168 -->

<!-- source-page: 169 -->

# 6.3.2 IMPLICIT DYNAMIC ANALYSIS USING DIRECT INTEGRATION

Products: Abaqus/Standard Abaqus/CAE

# References

• “Defining an analysis,” Section 6.1.2   
• “Dynamic analysis procedures: overview,” Section 6.3.1   
• \*DYNAMIC   
• “Configuring a dynamic, implicit procedure” in “Configuring general analysis procedures,” Section 14.11.1 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

# Overview

A direct-integration dynamic analysis in Abaqus/Standard:

• must be used when nonlinear dynamic response is being studied;   
• can be fully nonlinear (general dynamic analysis) or can be based on the modes of the linear system (subspace projection method); and   
• can be used to study a variety of applications, including:

– dynamic responses requiring transient fidelity and involving minimal energy dissipation;   
– dynamic responses involving nonlinearity, contact, and moderate energy dissipation; and   
quasi-static responses in which considerable energy dissipation provides stability and improved convergence behavior for determining an essentially static solution.

# General dynamic analysis

General nonlinear dynamic analysis in Abaqus/Standard uses implicit time integration to calculate the transient dynamic or quasi-static response of a system. The procedure can be applied to a broad range of applications calling for varying numerical solution strategies, such as the amount of numerical damping required to obtain convergence and the way in which the automatic time incrementation algorithm proceeds through the solution. Typical dynamic applications fall into three categories:

• Transient fidelity applications, such as an analysis of satellite systems, require minimal energy dissipation. In these applications small time increments are taken to accurately resolve the vibrational response of the structure, and numerical energy dissipation is kept at a minimum. These stringent requirements tend to degrade convergence behavior for simulations involving contact or nonlinearities.   
• Moderate dissipation applications encompass a more general range of dynamic events in which a moderate amount of energy is dissipated by plasticity, viscous damping, or other effects. Typical applications include various insertion, impact, and forming analyses. The response of these structures can be either monotonic or nonmonotonic. Accurate resolution of high-frequency

<!-- source-page: 170 -->

vibrations is usually not of interest in these applications. Some numerical energy dissipation tends to reduce solution noise and improve convergence behavior in these applications without significantly degrading solution accuracy.

• Quasi-static applications are primarily interested in determining a final static response. These problems typically show monotonic behavior, and inertia effects are introduced primarily to regularize unstable behavior. For example, the statically unstable behavior may be due to temporarily unconstrained rigid body modes or “snap-through” phenomena. Large time increments are taken when possible to obtain the final solution at minimal computational cost. Considerable numerical dissipation may be required to obtain convergence during certain stages of the loading history.

An example of a transient fidelity application is available in “Modeling of an automobile suspension,” Section 2.1.7 of the Abaqus Example Problems Guide. An analysis that includes both a moderate dissipation step and a quasi-static step is described in “Impact analysis of a pawl-ratchet device,” Section 2.1.17 of the Abaqus Example Problems Guide.

# Specifying the application type

Based on the classifications listed above, you should indicate the type of application you are studying when performing a general dynamic analysis. Abaqus/Standard assigns numerical settings based on your classification of the application type, and this classification can significantly affect a simulation. In some cases accurate results can be obtained with more than one application-type setting, in which case analysis efficiency should be considered. A general trend is that—among the three classifications—the high-dissipation quasi-static classification tends to result in the best convergence behavior and the lowdissipation transient fidelity classification tends to have the highest likelihood of convergence difficulty.

<table><tr><td>Input File Usage:</td><td>Use the following option for transient fidelity applications:*DYNAMIC, APPLICATION=TRANSIENT FIDELITY (default for models without contact)Use the following option for moderate dissipation applications:*DYNAMIC, APPLICATION=MODERATE DISSIPATION (default for models with contact)Use the following option for quasi-static applications:*DYNAMIC, APPLICATION=QUASI-STATIC</td></tr></table>

<table><tr><td>Abaqus/CAE Usage:</td><td>Step module: Create Step: General: Dynamic, ImplicitThe application type is specified in the Edit Step dialog box:Basic: Application: Transient fidelity, Moderate dissipation, Quasi-static, or Analysis product default</td></tr></table>

# Diagnostics for modeling errors associated with mass properties

Accurate representation of inertia properties is necessary for accurate dynamic analyses. In some cases Abaqus/Standard provides diagnostic messages when it detects likely modeling errors associated with the