About Dynamic Analysis Procedures

Implicit Versus Explicit Dynamics

The direct-integration dynamic procedure provided in Abaqus/Standard offers a choice of implicit operators for integration of the equations of motion, while Abaqus/Explicit uses the central-difference operator. In an implicit dynamic analysis, the integration operator matrix must be inverted and a set of nonlinear equilibrium equations must be solved at each time increment. In an explicit dynamic analysis, displacements and velocities are calculated in terms of quantities that are known at the beginning of an increment; therefore, the global mass and stiffness matrices need not be formed and inverted, which means that each increment is relatively inexpensive compared to the increments in an implicit integration scheme. The size of the time increment in an explicit dynamic analysis is limited, however, because the central-difference operator is only conditionally stable; whereas the implicit operator options available in Abaqus/Standard are unconditionally stable and, thus, there is no such limit on the size of the time increment that can be used for most analyses in Abaqus/Standard (accuracy governs the time increment in Abaqus/Standard).

The stability limit for the central-difference method (the largest time increment that can be taken without the method generating large, rapidly growing errors) is closely related to the time required for a stress wave to cross the smallest element dimension in the model; thus, the time increment in an explicit dynamic analysis can be very short if the mesh contains small elements or if the stress wave speed in the material is very high. The method is, therefore, computationally attractive for problems in which the total dynamic response time that must be modeled is only a few orders of magnitude longer than this stability limit; for example, wave propagation studies or some “event and response” applications. Many of the advantages of the explicit procedure also apply to slower (quasi-static) processes for cases in which it is appropriate to use mass scaling to reduce the wave speed (see Mass Scaling).

Abaqus/Explicit offers fewer element types than Abaqus/Standard. For example, only first-order, displacement method elements (4-node quadrilaterals, 8-node bricks, etc.) and modified second-order elements are used, and each degree of freedom in the model must have mass or rotary inertia associated with it. However, the method provided in Abaqus/Explicit has some important advantages:

The analysis cost rises only linearly with problem size, whereas the cost of solving the nonlinear equations associated with implicit integration rises more rapidly than linearly with problem size. Therefore, Abaqus/Explicit is attractive for very large problems.
The explicit integration method is often more efficient than the implicit integration method for solving extremely discontinuous short-term events or processes.
Problems involving stress wave propagation can be far more efficient computationally in Abaqus/Explicit than in Abaqus/Standard.

In choosing an approach to a nonlinear dynamic problem, you must consider the length of time for which the response is sought compared to the stability limit of the explicit method; the size of the problem; and the restriction of the explicit method to first-order, pure displacement method or modified second-order elements. In some cases the choice is obvious, but in many problems of practical interest the choice depends on details of the specific case. Experience is then the only useful guide.

Direct-Solution Versus Modal Superposition Procedures

Direct solution procedures must be used for dynamic analyses that involve a nonlinear response. Modal superposition procedures are a cost-effective option for performing linear or mildly nonlinear dynamic analyses.

Direct-Solution Dynamic Analysis Procedures

The following direct-solution dynamic analyses procedures are available in Abaqus:

Implicit dynamic analysis: Implicit direct-integration dynamic analysis (Implicit Dynamic Analysis Using Direct Integration) is used to study (strongly) nonlinear transient dynamic response in Abaqus/Standard.
Subspace-based explicit dynamic analysis: The subspace projection method in Abaqus/Standard uses direct, explicit integration of the dynamic equations of equilibrium written in terms of a vector space spanned by a number of eigenvectors (Implicit Dynamic Analysis Using Direct Integration). The eigenmodes of the system extracted in a frequency extraction step are used as the global basis vectors. This method can be very effective for systems with mild nonlinearities that do not substantially change the mode shapes. It cannot be used in contact analyses.
Explicit dynamic analysis: Explicit direct-integration dynamic analysis (Explicit Dynamic Analysis) is available in Abaqus/Explicit.
Direct-solution steady-state harmonic response analysis: The steady-state harmonic response of a system can be calculated in Abaqus/Standard directly in terms of the physical degrees of freedom of the model (Direct-Solution Steady-State Dynamic Analysis). The solution is given as in-phase (real) and out-of-phase (imaginary) components of the solution variables (displacement, stress, etc.) as functions of frequency. The main advantage of this method is that frequency-dependent effects (such as frequency-dependent damping) can be modeled. The direct method is the most accurate but also the most expensive steady-state harmonic response procedure. The direct method can also be used if nonsymmetric terms in the stiffness are important or if model parameters depend on frequency.

Modal Superposition Procedures

Abaqus includes a full range of modal superposition procedures. Modal superposition procedures can be run using a high-performance linear dynamics software architecture called SIM. The SIM architecture offers advantages over the traditional linear dynamics architecture for some large-scale analyses, as discussed below in Using the SIM Architecture for Modal Superposition Dynamic Analyses.

Prior to any modal superposition procedure, the natural frequencies of a system must be extracted using the eigenvalue analysis procedure (Natural Frequency Extraction). Frequency extraction can be performed using the SIM architecture.

The following modal superposition procedures are available in Abaqus:

Mode-based steady-state harmonic response analysis: A steady-state dynamic analysis based on the natural modes of the system can be used to calculate a system's linearized response to harmonic excitation (Mode-Based Steady-State Dynamic Analysis). This mode-based method is typically less expensive than the direct method. The solution is given as in-phase (real) and out-of-phase (imaginary) components of the solution variables (displacement, stress, etc.) as functions of frequency. Mode-based steady-state harmonic analysis can be performed using the SIM architecture.
Subspace-based steady-state harmonic response analysis: In this type of Abaqus/Standard analysis, the steady-state dynamic equations are written in terms of a vector space spanned by a number of eigenvectors (Subspace-Based Steady-State Dynamic Analysis). The eigenmodes of the system extracted in a frequency extraction step are used as the global basis vectors. The method is attractive because it allows frequency-dependent effects to be modeled and is much cheaper than the direct analysis method (Direct-Solution Steady-State Dynamic Analysis). Subspace-based steady-state harmonic response analysis can be used if the stiffness is nonsymmetric and can be performed using the SIM architecture.
Mode-based transient response analysis: The modal dynamic procedure (Transient Modal Dynamic Analysis) provides transient response for linear problems using modal superposition. Mode-based transient analysis can be performed using the SIM architecture.
Response spectrum analysis: A linear response spectrum analysis (Response Spectrum Analysis) is often used to obtain an approximate upper bound of the peak significant response of a system to a user-supplied input spectrum (such as earthquake data) as a function of frequency. The method has a very low computational cost and provides useful information about the spectral behavior of a system. Response spectrum analysis can be performed using the SIM architecture.
Random response analysis: The linearized response of a model to random excitation can be calculated based on the natural modes of the system (Random Response Analysis). This procedure is used when the structure is excited continuously and the loading can be expressed statistically in terms of a “Power Spectral Density” (PSD) function. The response is calculated in terms of statistical quantities such as the mean value and the standard deviation of nodal and element variables. Random response analysis can be performed using the SIM architecture.
Complex eigenvalue extraction: The complex eigenvalue extraction procedure performs eigenvalue extraction to calculate the complex eigenvalues and the corresponding complex mode shapes of a system (Complex Eigenvalue Extraction). The eigenmodes of the system extracted in a frequency extraction step are used as the global basis vectors. The complex eigenvalue extraction can be performed using the SIM architecture.

Using the SIM Architecture for Modal Superposition Dynamic Analyses

SIM is a high-performance software architecture available in Abaqus that can be used to perform modal superposition dynamic analyses. The SIM architecture is much more efficient than the traditional architecture for large-scale linear dynamic analyses (both model size and number of modes) with minimal output requests.

SIM-based analyses can be used to efficiently handle nondiagonal damping generated from element or material contributions, as discussed below in Damping in a Mode-Based Steady-State and Transient Linear Dynamic Analysis Using the SIM Architecture. Therefore, SIM-based procedures are an efficient alternative to subspace-based linear dynamic procedures for models with element damping or frequency-independent materials.

Activating the SIM Architecture

To use the SIM architecture for a modal superposition dynamic analysis, activate SIM for the initial frequency extraction procedure. SIM-based frequency extraction procedures write the mode shapes and other modal system information to a special linear dynamics data (.sim) file. By default, this data file is written to the scratch directory and deleted upon job completion; however, if restart is requested, the file is saved in the user directory. All subsequent mode-based steady-state or transient dynamic steps in an analysis automatically use this linear dynamics data file (and by extension the SIM architecture). If you restart an analysis that uses the SIM architecture, you must include the linear dynamics data file.

For more information about frequency extraction procedures, see Natural Frequency Extraction.

Input File Usage

FREQUENCY, SIM

Abaqus/CAE Usage

Step module: StepCreate: Frequency:  Use SIM-based linear dynamics procedures

Example

The SIM architecture will be used for the entire linear dynamic analysis in the following input file template:

STEP
FREQUENCY, EIGENSOLVER=LANCZOS, SIM
Data line to control eigenvalue extraction
COMPOSITE MODAL DAMPING
Data lines to define fraction of critical damping
END STEP
**
STEP
MODAL DYNAMIC
Data line to control time incrementation
SELECT EIGENMODES
Data lines to define the applicable mode ranges
MODAL DAMPING, VISCOUS=COMPOSITE
Data lines to define composite modal damping
END STEP
**
STEP
STEADY STATE DYNAMICS
Data lines to specify frequency ranges and bias parameters
SELECT EIGENMODES
Data lines to define the applicable mode ranges
END STEP
**
STEP
STEADY STATE DYNAMICS, SUBSPACE PROJECTION
Data lines to specify frequency ranges and bias parameters
SELECT EIGENMODES
Data lines to define the applicable mode ranges
END STEP

Output in a SIM-Based Analysis

Output is a fundamental factor in the performance of a linear dynamic analysis. Since it is difficult to predict the desired output quantities for a linear dynamic analysis, preselected output requests are ignored in SIM-based modal superposition procedures (except complex eigenvalue extraction). You must always specify output requests to the output database (.odb) file; otherwise, the analysis will not be performed.

There are several restrictions on available output requests that apply specifically to SIM-based analyses:

You cannot request output to the results (.fil) file.
Element variables cannot be output to the printed data (.dat) file except for random response analysis.

Limitations of the SIM Architecture

The cyclic symmetry modeling feature cannot be used in SIM-based analyses.

Reaction Force Calculations in Mode-Based Dynamic Analyses

In modal procedures that do not use SIM-based analysis, the reaction force calculation is based on the modal reaction forces extracted in the frequency extraction procedure. This approach does not take into account nondiagonal mass matrix and damping matrix contributions to the reaction force (as in the case of structural elements or substructures). Therefore, it might give rise to incorrect reaction force results. It is recommended that you use the steady-state dynamic or transient dynamic procedures based on the SIM architecture.

Nonphysical Material Properties in Dynamic Analyses

Abaqus relies on user-supplied model data and assumes that the material's physical properties reflect experimental results. Examples of meaningful material properties are a positive mass density per volume, a positive Young's modulus, and a positive value for any available damping coefficients. However, in special cases you might want to “adjust” a value of density, mass, stiffness, or damping in a region or a part of the model to bring the overall mass, stiffness, or damping to the expected required levels. Certain material options in Abaqus allow you to introduce nonphysical material properties to achieve this adjustment.

For example, to adjust the mass of the model, you can define a nonstructural mass with a negative mass value, use mass elements with a negative mass over a region of nodes, or introduce additional elements with negative density. Similarly, to adjust damping levels, you can use negative damping coefficients or introduce dashpot elements with a negative dashpot constant to reduce the overall damping levels. Springs with negative stiffness can be defined to adjust the model stiffness.

If you specify nonphysical but allowed material properties, Abaqus issues a warning message. However, if you specify nonphysical material properties that are not allowed, Abaqus issues an error message. When introducing nonphysical material properties, you must be aware that the overall behavior should be “physical”; for example, the mass values at all nodes must be positive in an eigenvalue extraction procedure.

There are consequences of using nonphysical material properties that are easy to check and interpret, and there are others beyond the control of Abaqus. Therefore, you should fully understand the stated problem and the consequences of using nonphysical material properties before you specify the properties. This is particularly important in Abaqus/Explicit analyses, where the size of the time increment depends on material properties. For example, distributed mass-dependent loads are calculated based on the overall mass density (positive and negative) provided.

Damping in Dynamic Analysis

Every nonconservative system exhibits some energy loss that is attributed to material nonlinearity, internal material friction, or to external (mostly joint) frictional behavior. Conventional engineering materials like steel and high strength aluminum alloys provide small amounts of internal material damping, not enough to prevent large amplification at or near resonant frequencies. Damping properties increase in modern composite fiber-reinforced materials, where the energy loss occurs through plastic or viscoelastic phenomena as well as from friction at the interfaces between the matrix and reinforcement. Still larger material damping is exhibited by thermoplastics. Mechanical dampers can be added to models to introduce damping forces to the system. In general, it is difficult to quantify the source of a system's damping. It usually comes from several sources simultaneously; for example, from energy loss during hysteretic loading, viscoelastic material properties, and external joint friction.

Users that work with a specific system know the source of the energy loss from experience. A variety of methods are available in Abaqus to specify damping that accurately models the energy loss in a dynamic system.

Sources of Damping

Abaqus has four categories of damping sources: material and element damping, global damping, modal damping, and damping associated with time integration. If necessary, you can include multiple damping sources and combine different damping sources in a model.

Material and Element Damping

Damping can be specified as part of a material definition that is assigned to a model (see Material Damping). In addition, Abaqus has elements such as dashpots, springs with their complex stiffness matrix, and connectors that serve as dampers, all with viscous and structural damping factors. Viscous damping can be included in mass, beam, pipe, and shell elements with general section properties; and it can also be used in substructure elements (see Generating Substructures). In direct steady-state dynamic analysis, you can define the viscous and structural damping due to the interaction between the contacting surfaces by using user subroutine UINTER (see UINTER). Contact damping is not applicable for linear perturbation procedures.

In acoustic elements, velocity proportional viscous damping is implemented using the volumetric drag parameter (see Acoustic Medium). Acoustic infinite elements and impedance conditions also add damping to a model.

Global Damping

In situations where material or element damping is not appropriate or sufficient, you can apply abstract damping factors to an entire model. Abaqus allows you to specify global damping factors for both viscous (Rayleigh damping) and structural damping (imaginary stiffness matrix).

Modal Damping

Modal damping applies only to mode-based linear dynamic analyses. This technique allows you to apply damping directly to the modes of the system. By definition, modal damping contributes only diagonal entries to the modal system of equations and can be defined several different ways.

Damping Associated with Time Integration

Marching through a simulation with a finite time increment size causes some damping. This type of damping applies only to analyses using direct time integration. See Implicit Dynamic Analysis Using Direct Integration for further discussion of this source of damping.

Damping in a Linear Dynamic Analysis

Damping can be applied to a linear dynamic system in two forms:

velocity proportional viscous damping; and
displacement proportional structural damping, which is for use in frequency domain dynamics. The exception is SIM-based transient modal dynamic analysis, where the structural damping is converted to the equivalent diagonal viscous damping (see Modal dynamic analysis).

An additional type of damping known as composite damping serves as a means to calculate a model average critical damping with the material density as the weight factor and is intended for use in mode-based dynamics (excluding subspace projection steady-state analysis). For more information, see Damping options for modal dynamics.

The types of damping available for linear dynamic analyses depend on the procedure type and the architecture (traditional or SIM) used to perform the analysis, as outlined in Table 1 and Table 2. For completeness, Table 1 also includes the damping options for a direct steady-state dynamic analysis. In addition to directly specified modal damping, global damping can be used in all linear dynamic procedures. Material and element damping can be used in subspace-based and SIM-based linear dynamic procedures.

Table 1. Damping sources for traditional architecture.
Traditional Architecture	Damping Source
Traditional Architecture	Modal	Global	Material and Element
Mode-based steady-state dynamics	$\sqrt$	$\sqrt$
Subspace-based steady-state dynamics		$\sqrt$	$\sqrt$
Transient modal dynamics	$\sqrt$	$\sqrt$
Random response analysis	$\sqrt$	$\sqrt$
Complex frequency		$\sqrt$	$\sqrt$
Response spectrum	$\sqrt$	$\sqrt$
Direct steady-state dynamics		$\sqrt$	$\sqrt$

Table 2. Damping sources for SIM architecture.
SIM Architecture	Damping Source
SIM Architecture	Modal	Global	Material and Element
Mode-based steady-state dynamics	$\sqrt$	$\sqrt$	$\sqrt$
Subspace-based steady-state dynamics	$\sqrt$	$\sqrt$	$\sqrt$
Transient modal dynamics	$\sqrt$	$\sqrt$	$\sqrt$
Random response analysis	$\sqrt$	$\sqrt$
Complex frequency	$\sqrt$	$\sqrt$	$\sqrt$
Response spectrum	$\sqrt$	$\sqrt$

In a subspace-based or SIM-based linear dynamic analysis, material and element damping operators must first be projected onto the basis of mode shapes. This projection results in a full modal damping matrix for both viscous and structural damping; therefore, a modal steady-state response analysis requires the solution of a system of linear equations at each frequency point. The size of this system is equal to the number of modes used in the response calculation. In a mode-based transient analysis, the projected damping operator is treated explicitly in time by including it on the right-hand side of the system of equations.

Frequency-dependent damping is supported only for the subspace-based and direct-integration steady-state dynamic procedures.

Material and element damping is not supported for the response spectrum or the random response procedures. In these procedures, only modal and global damping are allowed, and material or element damping is ignored.

Damping in a Mode-Based Steady-State and Transient Linear Dynamic Analysis Using the SIM Architecture

SIM-based linear dynamic analyses may include material and element damping contributions that introduce both diagonal and nondiagonal terms in the modal system of equations. The projection of material and element damping operators onto the basis of mode shapes is performed during the natural frequency extraction procedure, which enables a high-performance projection operation to be performed when used with the AMS eigensolver. If the damping operators depend on frequency, they will be evaluated at the frequency specified for property evaluation during the frequency extraction procedure.

When the structural and viscous damping operators are projected onto the mode shapes, the full modal damping matrix is stored in the linear dynamics data (.sim) file. The full modal damping matrix is combined with any diagonal contributions from global damping or traditional modal damping. The combined damping operator matrix is included in subsequent mode-based transient or steady-state dynamics steps. If there are nondiagonal (that is, projected) damping contributions and a large number of modes are included, performance of the linear dynamics calculations will be impacted since a direct solve must be performed at each frequency point.

Acoustic damping due to impedance conditions is projected onto the subspace of acoustic eigenvectors. These contributions are taken into account in a subspace-based steady-state dynamics analysis that uses the SIM architecture.

The default behavior for a SIM-based frequency extraction step is to project any element and material damping onto the mode shapes. You can turn off this damping projection if it is not desired; however, in this case only diagonal damping is available for subsequent modal superposition steps. If the projected damping matrices are not desired in a particular mode-based linear dynamic step for performance reasons, they can be deactivated in that step using the damping control techniques discussed above in Damping in Dynamic Analysis.

Input File Usage

Use the following option to project material and element damping operators in a SIM-based analysis:

FREQUENCY, SIM, DAMPING PROJECTION=ON (default)

Use the following option to turn off damping projection in a SIM-based analysis:

FREQUENCY, SIM, DAMPING PROJECTION=OFF

Abaqus/CAE Usage

To control the projection of element and material damping in a SIM-based frequency extraction step that uses the Lanczos eigensolver:

Step module: StepCreate: Frequency: Eigensolver: Lanczos, Use SIM-based linear dynamics procedures, toggle Project damping operators

To control the projection of element and material damping in a frequency extraction step that uses the AMS eigensolver:

Step module: StepCreate: Frequency: Eigensolver: AMS, toggle Project damping operators

Defining Viscous Damping

Abaqus allows you to choose a particular source of viscous damping, to add several sources, or to exclude viscous damping effects.

Defining Material/Element Viscous Damping

You can choose to model the viscous damping matrix, $D_{v i s c o u s}^{e l}$ , by using material damping properties and/or damping elements (such as dashpot or mass elements). The viscous, mass, and/or stiffness proportional damping matrix will include the material Rayleigh damping factors, $α_{R}^{m a t}$ and $β_{R}^{m a t}$ , as well as the element-oriented damping factor, $α_{R}^{e l}$ (for example, for mass elements). The material/element-based viscous damping matrix can be written as

\begin{matrix} D_{v i s c o u s}^{e l} & ​ = \sum_{e l = 1}^{N u m e l e m s} \int_{V} α_{R}^{m a t} N^{T} N ρ d v + \sum_{e l = 1}^{N u m e l e m s} α_{R}^{e l} m^{e l} \\ + \sum_{e l = 1}^{N u m e l e m s} \int_{V} β_{R}^{m a t} B^{T} D B d v + \sum_{e l = 1}^{N u m e l e m s} d_{v i s c o u s}^{e l}, \end{matrix}

where $d_{v i s c o u s}^{e l}$ represents the viscous damping matrix for elements such as dashpots. In mode-based procedures projection of $D_{v i s c o u s}^{e l}$ into the eigenmodes results in a nondiagonal matrix.

Input File Usage

Use the following option to specify material viscous damping for elements with mechanical degrees of freedom:

DAMPING, ALPHA= $α_{R}^{m a t}$ , BETA= $β_{R}^{m a t}$

Use the following option to specify material viscous damping for acoustic elements:

ACOUSTIC MEDIUM, VOLUMETRIC DRAG

Abaqus/CAE Usage

Property module: material editor: MechanicalDamping: Alpha:  $α_{R}^{m a t}$  or Beta:  $β_{R}^{m a t}$

Property module: material editor: OtherAcoustic Medium: Volumetric Drag

Defining Global Viscous Damping

You can supply global mass and stiffness proportional viscous damping factors, $α_{g l o b a l}$ and $β_{g l o b a l}$ , respectively, to create the global damping matrix using the global model mass and stiffness matrices, $M$ and $K$ , respectively:

D_{v i s c o u s}^{g} = α_{g l o b a l} M + β_{g l o b a l} K .

These parameters 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 viscous damping:

GLOBAL DAMPING, ALPHA= $α_{g l o b a l}$ , BETA= $β_{g l o b a l}$

Abaqus/CAE Usage

Global viscous damping is not supported in Abaqus/CAE.

Defining Viscous Modal Damping

Rayleigh damping introduces a damping matrix, $[C]$ , defined as

[C] = α [M] + β [K],

where $[M]$ is the mass matrix of the model, $[K]$ is the stiffness matrix of the model, and $α$ and $β$ are factors that you define.

In Abaqus/Standard you can define $α$ and $β$ independently for each mode, so that the above equation becomes

c_{M} = α_{M} m_{M} + β_{M} k_{M} (no sum on M),

where the subscript M refers to the mode number and $c_{M}$ , $m_{M}$ , and $k_{M}$ are the damping, mass, and stiffness terms associated with the Mth mode.

Input File Usage

Use the following option to define Rayleigh damping by specifying mode numbers:

MODAL DAMPING, VISCOUS=RAYLEIGH, DEFINITION=MODE NUMBERS

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

MODAL DAMPING, VISCOUS=RAYLEIGH, DEFINITION=FREQUENCY RANGE

Abaqus/CAE Usage

Use the following input to define Rayleigh damping by specifying mode numbers:

Step module: Create Step: Linear perturbation: any valid step type: Damping: Specify damping over ranges of: Modes, Rayleigh: Use Rayleigh damping data

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

Step module: Create Step: Linear perturbation: any valid step type: Damping: Specify damping over ranges of: Frequencies, Rayleigh: Use Rayleigh damping data

Defining Viscous Modal Damping as a Fraction of the Critical Damping

You can also specify the damping in each eigenmode in the model or for the specified frequency as a fraction of the critical damping. Critical damping is defined as

c_{c r} = 2 \sqrt{m k},

where m is the mass of the system and k is the stiffness of the system. Typical values of the fraction of critical damping, $ξ_{i}$ , are from 1% to 10% of critical damping, $c_{c r}$ ; but Abaqus/Standard accepts any positive value. The critical damping factors can be changed from step to step.

Input File Usage

Use the following option to define the fraction of critical damping by specifying mode numbers:

MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING, 
DEFINITION=MODE NUMBERS

Use the following option to define the fraction of critical damping by specifying a frequency range:

MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING, 
DEFINITION=FREQUENCY RANGE

Abaqus/CAE Usage

Use the following input to define the fraction of critical damping by specifying mode numbers:

Step module: Create Step: Linear perturbation: any valid step type: Damping: Specify damping over ranges of: Modes, Direct modal: Use direct damping data

Use the following input to define the fraction of critical damping by specifying frequency ranges:

Step module: Create Step: Linear perturbation: any valid step type: Damping: Specify damping over ranges of: Frequencies, Direct modal: Use direct damping data

Viscous Modal Damping for Uncoupled Structural-Acoustic Frequency Extractions

For uncoupled structural-acoustic frequency extractions performed using the AMS eigensolver, you can apply different damping to the structural and acoustic modes. This technique can be used only when damping is specified for a range of frequencies.

Input File Usage

Use the following option to apply the specified damping to only the structural modes:

MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING, 
DEFINITION=FREQUENCY RANGE, FIELD=MECHANICAL

Use the following option to apply the specified damping to only the acoustic modes:

MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING, 
DEFINITION=FREQUENCY RANGE, FIELD=ACOUSTIC

Use the following option to apply the specified damping to both structural and acoustic modes (default):

MODAL DAMPING, VISCOUS=FRACTION OF CRITICAL DAMPING, 
DEFINITION=FREQUENCY RANGE, FIELD=ALL

Abaqus/CAE Usage

The ability to specify different damping for structural and acoustic modes is not supported in Abaqus/CAE.

Controlling the Sources of Viscous Damping

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

D_{v i s c o u s} = D_{v i s c o u s}^{e l} + D_{v i s c o u s}^{g} .

Input File Usage

Use the following option to activate only the material/element viscous damping matrix:

DAMPING CONTROLS, VISCOUS=ELEMENT

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

DAMPING CONTROLS, VISCOUS=FACTOR

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

DAMPING CONTROLS, VISCOUS=COMBINED

Abaqus/CAE Usage

Damping controls are not supported in Abaqus/CAE.

Excluding Viscous Damping Effects

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

Input File Usage

Use the following option to exclude the viscous damping matrix:

DAMPING CONTROLS, VISCOUS=NONE

Abaqus/CAE Usage

Damping controls are not supported in Abaqus/CAE.

Defining Structural Damping

Abaqus allows you to choose a particular source of structural damping, to add several sources, or to exclude structural damping effects.

Defining Material/Element Structural Damping

The material/element structural damping matrix (that represents the imaginary stiffness and is proportional to forces or displacements) is defined as

K_{s}^{m} = \overset{N u m e l e m s}{\sum_{e l = 1}} \int_{V} s B^{T} D B d v + \overset{N u m e l e m s}{\sum_{e l = 1}} s^{e l} k^{e l},

where $s$ represents the material structural damping, $s^{e l}$ represents the structural damping coefficient for elements such as springs with complex stiffnesses and connectors, and $k^{e l}$ is the real element stiffness matrix. In mode-based procedures the projection of $K_{s}^{m}$ onto the mode shapes results in a full modal damping matrix. When using SIM-based modal procedures, the projected material and element damping matrix may be combined with global and modal damping (see Defining and Using Both Global and Modal Diagonal Damping below). Material/element structural damping is not available for acoustic elements.

Input File Usage

Use the following option to specify material structural damping:

DAMPING, STRUCTURAL= $s$

Abaqus/CAE Usage

Property module: material editor: MechanicalDamping: Structural:  $s$

Defining Global Structural Damping

You can define the global structural damping factor, $s_{g l o b a l}$ , to get

K_{s}^{g} = 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= $s_{g l o b a l}$

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 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

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 = Ω D_{v i s c o u s} + K_{s},

where $Ω$ 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.

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:

ξ_{α} = \frac{1}{m_{α}} ϕ_{α}^{T} (\sum_{m} ξ_{m} M_{m}) ϕ_{α},

where $ξ_{α}$ is the critical damping fraction used in mode $α$ , $ξ_{m}$ is the critical damping fraction defined for material m, $M_{m}$ is the mass matrix associated with material m, $ϕ_{α}$ is the eigenvector of mode $α$ , and $m_{α}$ is the generalized mass associated with mode $α$ :

m_{α} = ϕ_{α}^{T} M ϕ_{α} .

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

Input File Usage

Use both of the following options:

DAMPING, COMPOSITE= $ξ_{m}$  
MODAL DAMPING, VISCOUS=COMPOSITE

Abaqus/CAE Usage

Property module: material editor: MechanicalDamping: Composite:  $ξ_{m}$ 
Step module: Create Step: Linear perturbation: any valid step type: 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 except when you use the AMS eigensolver and request selective recovery. 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:

ξ_{α}^{M} = ϕ_{α}^{T} M_{ξ} ϕ_{α} = ϕ_{α}^{T} (\sum_{e l e m e n t s} ξ_{e l e m e n t}^{M} m_{e l e m e n t} + ξ_{\begin{matrix} m a t r i x \\ i n p u t \end{matrix}}^{M} M_{\begin{matrix} m a t r i x \\ i n p u t \end{matrix}}) ϕ_{α},

where $ξ_{α}^{M}$ is the mass weighted critical damping fraction used in mode $α$ , $M_{ξ}$ is a damped portion of the mass matrix, $ξ^{M}$ are fractions of critical damping for the element mass matrix and mass matrix input, and $ϕ_{α}$ is the eigenvector of mode $α$ .

The stiffness weighted damping per eigenmode is calculated as:

ξ_{α}^{K} = \frac{1}{ω_{α}^{2}} ϕ_{α}^{T} K_{ξ} ϕ_{α} = \frac{1}{ω_{α}^{2}} ϕ_{α}^{T} (\sum_{e l e m e n t s} ξ_{e l e m e n t}^{K} k_{e l e m e n t} + ξ_{\begin{matrix} m a t r i x \\ i n p u t \end{matrix}}^{K} K_{\begin{matrix} m a t r i x \\ i n p u t \end{matrix}}) ϕ_{α},

where $ξ_{α}^{K}$ is the stiffness weighted critical damping fraction used in mode $α$ , $K_{ξ}$ is a damped portion of the stiffness matrix, $ξ^{K}$ are fractions of critical damping for the element stiffness and matrix input stiffness, and $ϕ_{α}$ is the eigenvector of mode $α$ .

Input File Usage

Use both of the following options to specify composite modal damping:

FREQUENCY, EIGENSOLVER=LANCZOS, SIM
COMPOSITE MODAL DAMPING

Use the following option to specify the fraction of critical damping for all mass matrices included in matrix input:

COMPOSITE MODAL DAMPING, MASS MATRIX INPUT

Use the following option to specify the fraction of critical damping for all stiffness matrices included in matrix input:

COMPOSITE MODAL DAMPING, STIFFNESS MATRIX INPUT

Abaqus/CAE Usage

Defining composite modal damping for analyses using the SIM architecture is not supported in Abaqus/CAE.

Defining Global Damping in Acoustic Models

If your model contains only acoustic elements, Abaqus applies any specified global damping to all the acoustic fields by default. Similarly, if your model contains only stress/displacement elements, Abaqus applies any specified global damping to all the displacement and rotation fields by default.

If your model contains both acoustic elements and stress/displacement elements, the analysis type determines how global damping is applied. You can apply global damping to all of the displacement, rotation, and acoustic fields; to only the acoustic fields; or to only the displacement and rotation fields in the following procedures:

Mode-based analyses using uncoupled modes and the default high-performance linear dynamics implementation during the frequency extraction
Subspace-based steady-state dynamic analyses using coupled modes
Direct steady-state analyses

You can apply global damping only to all of the displacement, rotation, and acoustic fields in the following procedures:

Steady-state dynamic analyses using coupled modes
Mode-based steady-state dynamic analyses using coupled acoustic-structural modes

Input File Usage

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:

GLOBAL DAMPING, FIELD=ACOUSTIC

Use the following option to apply global damping only to the displacement and rotation fields:

GLOBAL DAMPING, FIELD=MECHANICAL

Abaqus/CAE Usage

Global damping is not supported in Abaqus/CAE.

Defining Modal Damping in Acoustic Models

If your model contains only acoustic elements, Abaqus applies any specified modal damping to all the acoustic fields by default. Similarly, if your model contains only stress/displacement elements, Abaqus applies any specified modal damping to all the displacement and rotation fields by default.

If your model contains both acoustic elements and stress/displacement elements, you can apply modal damping to all of the displacement, rotation, and acoustic fields. However, you can apply modal damping to the displacement and rotation fields or the acoustic fields separately only when using uncoupled modes and the default high-performance linear dynamics implementation during the frequency extraction.

Input File Usage

Use the following option to apply modal damping to all of the displacement, rotation, and acoustic fields in a model:

MODAL DAMPING, FIELD=ALL (default)

Use the following option to apply modal damping only to the acoustic fields:

MODAL DAMPING, FIELD=ACOUSTIC

Use the following option to apply modal damping only to the displacement and rotation fields:

MODAL DAMPING, FIELD=MECHANICAL

Abaqus/CAE Usage

Modal damping is not supported in Abaqus/CAE.

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.

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.

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 and Selecting the Modes on Which to Project).

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 https://support.3ds.com/knowledge-base/.

Alternatively, you can save the computed contribution factors in the output database (.odb) file. If you request history output, the computed acoustic contribution factors are saved as history curves in the output database. Field output is relevant only for the grid acoustic contribution factors. If you request field output for the grid acoustic contribution factors, their output into the SIM database file is blocked.

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:

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:

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:

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:

ACOUSTIC CONTRIBUTION, TYPE=LOAD

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. You can specify this set by giving the name of the node set containing the nodes on the acoustic-structural interface, or you can specify the set by giving the name of the surface containing the structural nodes on the acoustic-structural interface. If you use both methods simultaneously, the node set for computing panel acoustic contribution factors is imposed as the union of the node sets prescribed by each method. If this node set contains other structural or acoustic nodes that do not belong to the acoustic-structural interface, those 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:

ACOUSTIC CONTRIBUTION, TYPE=PANEL, 
STRUCTURAL NODES=structural_nset, SURFACE=structural_surface

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. You can specify this set by giving the name of the node set containing the nodes on the acoustic-structural interface, or you can specify the set by giving the name of the surface containing the structural nodes on the acoustic-structural interface. If you use both methods simultaneously, the node set for computing panel acoustic contribution factors is imposed as the union of the node sets prescribed by each method. If this node set contains other structural or acoustic nodes that do not belong to the acoustic-structural interface, these nodes are 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 1,000,000 nodes. If this number is exceeded, the first 1,000,000 nodes are used.

Input File Usage

Use the following option to compute the grid contribution factor:

ACOUSTIC CONTRIBUTION, TYPE=GRID,
STRUCTURAL NODES=structural_nset, SURFACE=structural_surface

Input File Usage

Use the following option to compute the grid contribution factor and output it as field output to the output database (.odb) file:

ACOUSTIC CONTRIBUTION, TYPE=GRID,
STRUCTURAL NODES=structural_nset, SURFACE=structural_surface, OUTPUT=FIELD

Abaqus/CAE Usage

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

Normal Velocity Output in Steady-State Dynamic Analysis

For metal structures in air, the forced response of the structure is largely uncoupled from the acoustic vibrations of the air in the frequency range of interest. On the other hand, the acoustic vibrations of the air are strongly driven by the structural motion. Therefore, it is common in engineering to estimate the noise radiated from a structure using only the surface normal velocity of the structure.

Abaqus/Standard can provide normal velocity field output at nodes of the element-based surface in a steady-state dynamic analysis (see Figure 1).

The following output variables are available:

VN: The complex-valued surface normal velocity defined as the projection of the nodal complex velocity vector along the local (real-valued) surface normal vector at the node. VN is itself vector-valued, carrying the direction of the normal.
VNSQ: The real-valued surface normal velocity squared, defined as the scalar (real) magnitude squared of the surface normal velocity vector.
AVNSQ: The area-weighted surface normal velocity squared, or the acoustic power normalized by the acoustic impedance of the surrounding fluid; that is, a real-valued scalar equal to VNSQ multiplied by the local surface area adjacent to the node.

Input File Usage

Use the following option to specify the element-based surface for the normal velocity output:

*NODE OUTPUT, SURFACE=element_based_surface_name
list of output variables

Abaqus/CAE Usage

Specifying the surface for the normal velocity output is not supported Abaqus/CAE.

Local Normal Stiffness Output In Eigenvalue Extraction Analysis

In the engineering design of structures such as airplanes and automobiles it is common to estimate how a certain panel or shell structure locally resists the normal loads. This allows you to indicate weak spots and optimize the design.

The local normal stiffness is defined as a ratio of the normal force and normal displacement magnitudes at a surface node, where the force is applied statically at the surface node in the surface normal direction and the displacement is obtained from the linear static analysis of the model loaded with that single normal force (see Figure 2).

Calculation of the local normal stiffness for a panel requires solving a linear static problem for every node at the panel surface. In practical simulations (when the number of surface nodes is in the hundreds of thousands or millions), this calculation becomes extremely intensive and is not practical. However, you can calculate the approximate local normal stiffness very effectively by using the mode superposition method.

Abaqus/Standard can provide local normal stiffness field output at nodes of the element-based surface in the eigenvalue extraction analysis. The local normal stiffness field output is associated with the last output frame in the eigenvalue extraction procedure.

The output variable for the nodal local normal stiffness is STIFN.

Input File Usage

Use the following option to specify the element-based surface for the local normal stiffness output:

*NODE OUTPUT, SURFACE=element_based_surface_name
STIFN

Abaqus/CAE Usage

Specifying the surface for the local normal stiffness output is not supported in Abaqus/CAE.

Parallel Execution of Steady-State Dynamic Analysis

Calculation of the frequency response for large finite element systems can be time consuming. Parallel execution is a practical option for steady-state dynamic analyses with millions of degrees of freedom, thousands of frequencies, and hundreds of load cases. For more information, see Parallel Execution of Steady-State Dynamic Analyses.