Natural Frequency Extraction

Eigenvalue Extraction

The eigenvalue problem for the natural frequencies of an undamped finite element model is

(- ω^{2} M^{M N} + K^{M N}) ϕ^{N} = 0,

where

$M^{M N}$: is the mass matrix (which is symmetric and positive definite);
$K^{M N}$: is the stiffness matrix (which includes initial stiffness effects if the base state included the effects of nonlinear geometry);
$ϕ^{N}$: is the eigenvector (the mode of vibration); and
M and N: are degrees of freedom.

When $K^{M N}$ is positive definite, all eigenvalues are positive. Rigid body modes and instabilities cause $K^{M N}$ to be indefinite. Rigid body modes produce zero eigenvalues. Instabilities produce negative eigenvalues and occur when you include initial stress effects. Abaqus/Standard solves the eigenfrequency problem only for symmetric matrices.

Selecting the Eigenvalue Extraction Method

Abaqus/Standard provides three eigenvalue extraction methods:

Lanczos
Automatic multilevel substructuring (AMS), an add-on analysis capability for Abaqus/Standard
Subspace iteration

In addition, you must consider the software architecture used for the subsequent modal superposition procedures. The choice of architecture has minimal impact on the frequency extraction procedure, but the default SIM architecture offers significant performance improvements over the traditional architecture for subsequent mode-based steady-state or transient dynamic procedures (see Using the SIM Architecture for Modal Superposition Dynamic Analyses). The architecture that you use for the frequency extraction procedure is used for all subsequent mode-based linear dynamic procedures; you cannot switch architectures during an analysis. For information about the software architectures used by the different eigensolvers, see Table 1.

Table 1. Software architectures available with different eigensolvers.
Software Architecture	Eigensolver
Software Architecture	Lanczos	AMS	Subspace Iteration
Traditional	$\sqrt$		$\sqrt$
SIM	$\sqrt$	$\sqrt$	$\sqrt$

The Lanczos solver with the SIM architecture is the default eigenvalue extraction method because it has the most general capabilities. However, the Lanczos method is generally slower than the AMS method. The increased speed of the AMS eigensolver is particularly evident when you require a large number of eigenmodes for a system with many degrees of freedom. However, the AMS method has the following limitations:

All restrictions imposed on SIM-based linear dynamic procedures also apply to mode-based linear dynamic analyses based on mode shapes computed by the AMS eigensolver. See Using the SIM Architecture for Modal Superposition Dynamic Analyses for details.
The AMS eigensolver does not compute composite modal damping factors when selective recovery is requested.
You cannot use the AMS eigensolver in an analysis that contains piezoelectric elements.
You cannot request output to the results (.fil) file in an AMS frequency extraction step.
The SIM-based architecture does not support the following capabilities: cyclic symmetry, fluid properties associated with an incident wave, transient dynamic procedures used for coupled structural-acoustic problems, symmetric model generation, and imperfections based on eigenmode data.
At least one output request is required to run analyses using the SIM-based architecture.

If your model has many degrees of freedom and these limitations are acceptable, you can use the AMS eigensolver. Otherwise, you can use the Lanczos eigensolver. For a description of the Lanczos eigensolver and the subspace iteration method, see Eigenvalue extraction.

Lanczos Eigensolver

For the Lanczos method, you must provide the maximum frequency of interest or the number of eigenvalues required; Abaqus/Standard determines a suitable block size (although you can override this choice, if required). If you specify both the maximum frequency of interest and the number of eigenvalues required and the actual number of eigenvalues is underestimated, Abaqus/Standard issues a corresponding warning message; the remaining eigenmodes are found by restarting the frequency extraction.

You can also specify the minimum frequencies of interest; Abaqus/Standard extracts eigenvalues until either it extracts the requested number of eigenvalues in the given range or it extracts all the frequencies in the given range.

See Using the SIM Architecture for Modal Superposition Dynamic Analyses for information on using the SIM architecture with the Lanczos eigensolver.

Input File Usage

FREQUENCY, EIGENSOLVER=LANCZOS

Abaqus/CAE Usage

Step module: StepCreate: Frequency: Basic: Eigensolver:  Lanczos

Choosing a Block Size for the Lanczos Method

In general, the block size for the Lanczos method can be as large as the largest expected multiplicity of eigenvalues (that is, the largest number of modes with the same frequency). A block size larger than 10 is not recommended. If the number of eigenvalues requested is n, the default block size is the minimum of (7, n). The choice of 7 for block size proves to be efficient for problems with rigid body modes. Abaqus/Standard typically determines the number of block Lanczos steps within each Lanczos run, but you can change the number. In general, if a particular type of eigenproblem converges slowly, providing more block Lanczos steps reduces the analysis cost. However, if you know that a particular type of problem converges quickly, providing fewer block Lanczos steps reduces the amount of in-core memory used. The default values are


Block size	Maximum number of block Lanczos steps
1	80
2	50
3	45
≥ 4	35

Automatic Multilevel Substructuring (AMS) Eigensolver

For the AMS method, you only need to specify the maximum frequency of interest (the global frequency), and Abaqus/Standard extracts all the modes up to this frequency. You can also specify the minimum frequencies of interest and the number of requested modes. However, specifying these values does not affect the number of modes extracted by the eigensolver; it affects only the number of modes that Abaqus/Standard stores for output or for a subsequent modal analysis.

You can control the execution of the AMS eigensolver by specifying three parameters: $A M S_{{cutoff}_{1}}$ , $A M S_{{cutoff}_{2}}$ , and $A M S_{{cutoff}_{3}}$ . These three parameters multiplied by the maximum frequency of interest define three cutoff frequencies. $A M S_{{cutoff}_{1}}$ (default value of 5) controls the cutoff frequency for substructure eigenproblems in the reduction phase, while $A M S_{{cutoff}_{2}}$ and $A M S_{{cutoff}_{3}}$ (default values of 1.7 and 1.1, respectively) control the cutoff frequencies used to define a starting subspace in the reduced eigensolution phase. Generally, increasing the value of $A M S_{{cutoff}_{2}}$ and $A M S_{{cutoff}_{3}}$ improves the accuracy of the results but might affect the performance of the analysis.

Requesting Eigenvectors at All Nodes

By default, the AMS eigensolver computes eigenvectors at every node of the model.

Input File Usage

FREQUENCY, EIGENSOLVER=AMS

Abaqus/CAE Usage

Step module: StepCreate: Frequency: Basic: Eigensolver: AMS

Requesting Eigenvectors Only at Specified Nodes

Alternatively, you can specify a node set. Abaqus/Standard computes partial eigenvectors and stores them only at the nodes that belong to the specified node set. Computing eigenvectors at only selected nodes improves performance and reduces the amount of stored data. Therefore, it is recommended that you use this option for large models.

The node set that you specify must include all nodes at which loads are applied and the nodes at which output is requested in the current natural frequency extraction analysis or in any subsequent modal analysis, including any restarted analysis. If element output is requested or element-based loading is applied, you must also include all nodes attached to the associated elements in this node set, including the internal nodes created by Abaqus/Standard. You cannot specify internal nodes to include in the node set. However, Abaqus/Standard automatically selects all the nodes that need to be included in the node set. This guarantees that all nodes required for the load application and output specified in the current analysis job are included in the node set. If loads are applied or output is requested at nodes not included in this node set in a restart analysis, Abaqus/Standard issues diagnostic messages and stops the restarted analysis. The following nodes are selected automatically:

nodes at which a concentrated load is applied in the mode-based procedures that follow this step,
nodes at which output is requested in the eigenvalue extraction analysis or in the mode-based procedures that follow this step,
nodes at which residual vectors are requested,
nodes of elements at which a distributed load is applied,
nodes of elements with frequency-dependent material properties, and
nodes of elements at which output is requested in the eigenvalue extraction analysis or in the mode-based procedures that follow this step.

Input File Usage

Use the following option to specify a node set:

FREQUENCY, EIGENSOLVER=AMS, NSET=name

Use the following option to allow Abaqus/Standard to select the nodes automatically:

FREQUENCY, EIGENSOLVER=AMS, NSET

Abaqus/CAE Usage

You can only request eigenvectors at specific nodes by specifying a node set in Abaqus/CAE.

Step module: StepCreate: Frequency: Basic: Eigensolver: AMS: Limit region of saved eigenvectors, select node set

Controlling the AMS Eigensolver

The AMS method consists of the following three phases:

Reduction phase

In this phase Abaqus/Standard uses a multilevel substructuring technique to reduce the full system in a way that allows a very efficient eigensolution of the reduced system. The approach combines a sparse factorization based on a multilevel supernode elimination tree and a local eigensolution at each supernode.

Starting from the lowest level supernodes, we use a Craig-Bampton substructure reduction technique to successively reduce the size of the system as we progress upward in the elimination tree. At each supernode a local eigensolution is obtained based on fixing the degrees of freedom connected to the next higher level supernode (these are the local retained or “fixed-interface” degrees of freedom). At the end of the reduction phase, the full system has been reduced such that the reduced stiffness matrix is diagonal and the reduced mass matrix has unit diagonal values but contains off-diagonal blocks of nonzero values representing the coupling between the supernodes.

The cost of the reduction phase depends on the system size and the number of eigenvalues extracted (the number of eigenvalues extracted is controlled indirectly by specifying the highest eigenfrequency required). You can make trade-offs between cost and accuracy during the reduction phase through the $A M S_{{cutoff}_{1}}$ parameter. This parameter multiplied by the highest eigenfrequency specified for the full model yields the highest eigenfrequency that is extracted in the local supernode eigensolution. Increasing the value of $A M S_{{cutoff}_{1}}$ increases the accuracy of the reduction since more local eigenmodes are retained. However, increasing the number of retained modes also increases the cost of the reduced eigensolution phase, which is discussed next.

Reduced eigensolution phase

In this phase Abaqus/Standard computes the eigensolution of the reduced system that comes from the previous phase. Although the reduced system typically is two orders of magnitude smaller in size than the original system, generally it still is too large to solve directly. Thus, the system is further reduced mainly by truncating the retained eigenmodes and then solved using a single subspace iteration step. The two AMS parameters, $A M S_{{cutoff}_{2}}$ and $A M S_{{cutoff}_{3}}$ , define a starting subspace of the subspace iteration step. The default values of these parameters are carefully chosen and provide accurate results in most cases. When a more accurate solution is required, the recommended procedure is to increase both parameters proportionally from their respective default values.

Recovery phase

In this phase the eigenvectors of the original system are recovered using eigenvectors of the reduced problem and local substructure modes. If you request recovery at specified nodes, the eigenvectors are computed only at those nodes.

Subspace Iteration Method

For the subspace iteration procedure, you only need to specify the number of eigenvalues required; Abaqus/Standard chooses a suitable number of vectors for the iteration. If the subspace iteration technique is requested, you can also specify the maximum frequency of interest; Abaqus/Standard extracts eigenvalues until either the requested number of eigenvalues has been extracted or the last frequency extracted exceeds the maximum frequency of interest.

Input File Usage

FREQUENCY, EIGENSOLVER=SUBSPACE

Abaqus/CAE Usage

Step module: StepCreate: Frequency: Basic: Eigensolver: Subspace

Structural-Acoustic Coupling

Structural-acoustic coupling affects the natural frequency response of systems. In Abaqus/Standard the AMS eigensolver and the Lanczos eigensolver can extract coupled modes to fully include this effect. The subspace eigensolver neglects the effect of coupling for computing the modes and frequencies; the modes and frequencies are computed using natural boundary conditions at the structural-acoustic coupling surface. By default, the same is done for the AMS eigensolver; the coupling is projected onto the modal space and stored for later use.

Structural-Acoustic Coupling Using the Lanczos Eigensolver

If structural-acoustic coupling is present in the model and the Lanczos method is used, Abaqus/Standard extracts the coupled modes by default. Because these modes fully account for coupling, they represent the mathematically optimal basis for subsequent modal procedures. The effect is most noticeable in strongly coupled systems such as steel shells and water. However, coupled structural-acoustic modes cannot be used in subsequent random response or response spectrum analyses. You can define the coupling using either acoustic-structural interaction elements (see Acoustic Interface Elements) or the surface-based tie constraint (see Acoustic, Shock, and Coupled Acoustic-Structural Analysis). It is possible to ignore coupling when extracting acoustic and structural modes; in this case the coupling boundary is treated as traction-free on the structural side and rigid on the acoustic side.

For frequency extractions that use the Lanczos eigensolver based on the SIM architecture, it is also possible to project structural-acoustic coupling operators onto the subspace of eigenvectors. The modes are computed using traction-free boundary conditions on the structural side of the coupling boundary and rigid boundary conditions on the acoustic side. Structural-acoustic coupling operators (see Acoustic, Shock, and Coupled Acoustic-Structural Analysis) are projected by default onto the subspace of eigenvectors. Contributions to these global operators, which come from surface-based tie constraints defined between structural and acoustic surfaces, are assembled into global matrices that are projected onto the mode shapes and used in subsequent SIM-based modal dynamic procedures.

Input File Usage

Use the following option to account for structural-acoustic coupling during the frequency extraction:

FREQUENCY, EIGENSOLVER=LANCZOS, 
ACOUSTIC COUPLING=ON (default)

Use the following option to project structural-acoustic coupling on the uncoupled eigenmodes during the frequency extraction:

FREQUENCY, EIGENSOLVER=LANCZOS, SIM,  
ACOUSTIC COUPLING=PROJECTION (only if the Lanczos eigensolver is based on the SIM architecture)

Use the following option to ignore structural-acoustic coupling during the frequency extraction:

FREQUENCY, EIGENSOLVER=LANCZOS, 
ACOUSTIC COUPLING=OFF

Abaqus/CAE Usage

Use the following option to account for structural-acoustic coupling during the frequency extraction:

Step module: StepCreate: Frequency: Basic: Eigensolver: Lanczos, toggle on Include acoustic-structural coupling where applicable

Use the following option to project structural-acoustic coupling on the uncoupled eigenmodes during the frequency extraction:

Step module: StepCreate: Frequency: Basic: Eigensolver: Lanczos, toggle on Use SIM-based linear dynamics procedures, toggle on Project acoustic-structural coupling where applicable

Use the following option to ignore structural-acoustic coupling during the frequency extraction:

Step module: StepCreate: Frequency: Basic: Eigensolver: Lanczos, toggle off Include acoustic-structural coupling where applicable

Structural-Acoustic Coupling Using the AMS Eigensolver

For frequency extractions that use the AMS eigensolver, the modes are computed by default using traction-free boundary conditions on the structural side of the coupling boundary and rigid boundary conditions on the acoustic side. Structural-acoustic coupling operators (see Acoustic, Shock, and Coupled Acoustic-Structural Analysis) are projected by default onto the subspace of eigenvectors. Contributions to these global operators, which come from surface-based tie constraints defined between structural and acoustic surfaces, are assembled into global matrices that are projected onto the mode shapes and used in subsequent SIM-based modal dynamic procedures.

For frequency extractions that use the AMS eigensolver, Abaqus/Standard can also extract the coupled modes. Because these modes fully account for coupling, they represent the mathematically optimal basis for subsequent modal procedures. The effect is most noticeable in strongly coupled systems such as steel shells and water. However, extracting the coupled structural-acoustic modes using the AMS eigensolver is computationally more expensive than the default option, where the coupling operators are projected onto the subspace of uncoupled eigenvectors.

User-defined acoustic-structural interaction elements (see Acoustic Interface Elements) cannot be used in an AMS eigenvalue extraction analysis.

Input File Usage

Use the following option to project structural-acoustic coupling operators onto the subspace of eigenvectors:

FREQUENCY, EIGENSOLVER=AMS, 
ACOUSTIC COUPLING=PROJECTION (default)

Use the following option to disable the projection of structural-acoustic coupling operators:

FREQUENCY, EIGENSOLVER=AMS, 
ACOUSTIC COUPLING=OFF

Use the following option to extract coupled structural-acoustic eigenmodes:

FREQUENCY, EIGENSOLVER=AMS, 
ACOUSTIC COUPLING=ON

Abaqus/CAE Usage

Use the following option to project structural-acoustic coupling operators onto the subspace of eigenvectors:

Step module: StepCreate: Frequency: Basic: Eigensolver: AMS, toggle on Project acoustic-structural coupling where applicable

Use the following option to disable the projection of structural-acoustic coupling operators:

Step module: StepCreate: Frequency: Basic: Eigensolver: AMS, toggle off Project acoustic-structural coupling where applicable

Requesting the coupled structural-acoustic modes during the AMS eigenanalysis is not supported in Abaqus/CAE.

Specifying a Frequency Range for the Acoustic Modes

Because structural-acoustic coupling can be ignored during the AMS and SIM-based Lanczos eigenanalysis, the computed resonances are, in principle, higher than those of the fully coupled system. This might be understood as a result of neglecting the mass of the fluid in the structural phase and vice versa. For the common metal and air case, the structural resonances might be relatively unaffected; however, some acoustic modes that are significant in the coupled response may be omitted due to the air's upward frequency shift during eigenanalysis. Therefore, Abaqus/Standard allows you to specify a multiplier, so that the maximum acoustic frequency in the analysis is taken to be higher than the structural maximum.

Input File Usage

Use either of the following options:

FREQUENCY, EIGENSOLVER=AMS
, , , , , , acoustic range factor

or

FREQUENCY, EIGENSOLVER=LANCZOS, SIM, 
ACOUSTIC COUPLING=PROJECTION
, , , , , , acoustic range factor

Abaqus/CAE Usage

Step module: StepCreate: Frequency: Basic: Eigensolver: AMS, Acoustic range factor: acoustic range factor

Specifying a frequency range for the acoustic modes during Lanczos eigenanalysis is not supported in Abaqus/CAE.

Effects of Fluid Motion on Natural Frequency Analysis of Acoustic Systems

To extract natural frequencies from an acoustic-only or coupled structural-acoustic system in which fluid motion is prescribed using an acoustic flow velocity, either the Lanczos method or the complex eigenvalue extraction procedure can be used. In the former case Abaqus/Standard extracts real-only eigenvalues and considers the fluid motion's effects only on the acoustic stiffness matrix. Thus, these results are of primary interest as a basis for subsequent linear perturbation procedures. When the complex eigenvalue extraction procedure is used, the fluid motion effects are included in their entirety; that is, the acoustic stiffness and damping matrices are included in the analysis.

Frequency Shift

For the Lanczos and subspace iteration eigensolvers you can specify a positive or negative shifted squared frequency, S. This feature is useful when a particular frequency is of concern or when the natural frequencies of an unrestrained structure or a structure that uses secondary base motions (large mass approach) are required. In the latter case a shift from zero (the frequency of the rigid body modes) avoids singularity problems or round-off errors for the large mass approach; a negative frequency shift is normally used. The default is no shift.

If the Lanczos eigensolver is in use and the user-specified shift is outside the requested frequency range, the shift is adjusted automatically to a value close to the requested range.

Normalization

For the Lanczos and subspace iteration eigensolvers both displacement and mass eigenvector normalization are available. If the non-SIM architecture is used, displacement normalization is the default. Mass normalization is the only option available for SIM-based natural frequency extraction.

The choice of eigenvector normalization type has no influence on the results of subsequent modal dynamic steps (see Linear analysis of a rod under dynamic loading). The normalization type determines only the manner in which the eigenvectors are represented.

In addition to extracting the natural frequencies and mode shapes, the Lanczos and subspace iteration eigensolvers automatically calculate the generalized mass, the participation factor, the effective mass, and the composite modal damping for each mode; therefore, these variables are available for use in subsequent linear dynamic analyses. The AMS eigensolver computes the generalized mass and the participation factor.

Displacement Normalization

If displacement normalization is selected, the eigenvectors are normalized so that the largest displacement entry in each vector is unity. If the displacements are negligible, as in a torsional mode, the eigenvectors are normalized so that the largest rotation entry in each vector is unity. In a coupled acoustic-structural extraction, if the displacements and rotations in a particular eigenvector are small when compared to the acoustic pressures, the eigenvector is normalized so that the largest acoustic pressure in the eigenvector is unity. The normalization is done before the recovery of dependent degrees of freedom that have been previously eliminated with multi-point constraints or equation constraints. Therefore, it is possible that such degrees of freedom might have values greater than unity.

Input File Usage

FREQUENCY, NORMALIZATION=DISPLACEMENT, SIM=NO

Abaqus/CAE Usage

Step module: StepCreate: Frequency: Other: Normalize eigenvectors by: Displacement

Mass Normalization

Alternatively, the eigenvectors can be normalized so that the generalized mass for each vector is unity.

The “generalized mass” associated with mode $α$ is

m_{α} = ϕ_{α}^{N} M^{N M} ϕ_{α}^{M} (no sum on α),

where $M^{N M}$ is the structure's mass matrix and $ϕ_{α}^{N}$ is the eigenvector for mode $α$ . The superscripts N and M refer to degrees of freedom of the finite element model.

If the eigenvectors are normalized with respect to mass, all the eigenvectors are scaled so that $m_{α}$ =1. For coupled acoustic-structural analyses, an acoustic contribution fraction to the generalized mass is computed as well.

Input File Usage

FREQUENCY, NORMALIZATION=MASS

Abaqus/CAE Usage

Step module: StepCreate: Frequency: Other: Normalize eigenvectors by: Mass

Modal Participation Factors

The participation factor for mode $α$ in direction i, $Γ_{α i}$ , is a variable that indicates how strongly motion in the global x-, y-, or z-direction or rigid body rotation about one of these axes is represented in the eigenvector of that mode. The six possible rigid body motions are indicated by $i = 1$ , 2, $\dots$ , 6. The participation factor is defined as

Γ_{α i} = \frac{1}{m_{α}} ϕ_{α}^{N} M^{N M} T_{i}^{M} (no sum on α),

where $T_{i}^{N}$ defines the magnitude of the rigid body response of degree of freedom N in the model to imposed rigid body motion (displacement or infinitesimal rotation) of type i. For example, at a node with three displacement and three rotation components, $T_{i}^{N}$ is

(\begin{matrix} 1 & 0 & 0 & 0 & (z - z_{0}) & - (y - y_{0}) \\ 0 & 1 & 0 & - (z - z_{0}) & 0 & (x - x_{0}) \\ 0 & 0 & 1 & (y - y_{0}) & - (x - x_{0}) & 0 \\ 0 & 0 & 0 & 1 & 0 & 0 \\ 0 & 0 & 0 & 0 & 1 & 0 \\ 0 & 0 & 0 & 0 & 0 & 1 \end{matrix}) {\begin{matrix} {\hat{e}}_{1} \\ {\hat{e}}_{2} \\ {\hat{e}}_{3} \\ {\hat{e}}_{4} \\ {\hat{e}}_{5} \\ {\hat{e}}_{6} \end{matrix}},

where ${\hat{e}}_{i}$ is unity and all other ${\hat{e}}_{p}$ are zero; x, y, and z are the coordinates of the node; and $x_{0}$ , $y_{0}$ , and $z_{0}$ represent the coordinates of the center of rotation. The participation factors are, thus, defined for the translational degrees of freedom and for rotation around the center of rotation. For coupled acoustic-structural eigenfrequency analysis, an additional acoustic participation factor is computed as outlined in Coupled acoustic-structural medium analysis.

Modal Effective Mass

The effective mass for mode $α$ associated with kinematic direction i ( $i = 1$ , 2, $\dots$ , 6) is defined as

m_{α i}^{eff} = {(Γ_{α i})}^{2} m_{α} (no sum on α) .

If the effective masses of all modes are added in any global translational direction, the sum should give the total mass of the model (except for mass at kinematically restrained degrees of freedom). Thus, if the effective masses of the modes used in the analysis add up to a value that is significantly less than the model's total mass, this result suggests that modes that have significant participation in a certain excitation direction have not been extracted.

For coupled acoustic-structural eigenfrequency analysis, an additional acoustic effective mass is computed as outlined in Coupled acoustic-structural medium analysis.

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. For more information, see Defining Composite Modal Damping.

Residual Modes

Several analysis types in Abaqus/Standard are based on the eigenmodes and eigenvalues of an undamped system. For example, in a mode-based steady-state dynamic analysis the mass, stiffness, and damping matrices and load vectors of the physical system are projected onto a set of eigenmodes. This projection results in a condensed (not necessarily diagonal) system of equations in terms of the modal amplitudes (or generalized degrees of freedom). The physical system response is obtained by scaling each eigenmode by its corresponding modal amplitude and superimposing the results (for more information, see Linear dynamic analysis using modal superposition).

Due to the computational cost, usually only a limited subset of the lower frequency eigenmodes of the system is extracted. Depending on the nature of the loading, the accuracy of the modal solution might suffer if too few higher frequency modes are used. To achieve sufficient accuracy using the available lower frequency eigenmodes, you can augment the modal subspace with additional modes known as residual modes. Residual modes help correct errors introduced by the modal basis truncation.

In Abaqus/Standard the residual mode vector is obtained from the linear static response of the finite element model to the nominal or scaled (for example, unit) load corresponding to the actual load applied in the mode-based analysis. The static solution is orthogonalized against the extracted eigenvectors and other residual mode vectors. The orthogonalization process automatically removes redundant linearly dependent vectors when constructing the basis of the modal subspace. As an outcome of the orthogonalization process, a pseudoeigenvalue corresponding to each residual mode is obtained as the Rayleigh ratio calculated for a residual mode shape vector.

Generally, the term eigenvalue is used in the Abaqus/Standard user assistance to refer to the actual eigenvalues and pseudoeigenvalues. All data (participation factors, etc.; see Output) associated with the modes (eigenmodes and residual modes) are ordered by increasing eigenvalue. Therefore, both eigenmodes and residual modes are assigned mode numbers. In the printed output in the data file, Abaqus/Standard clearly identifies which modes are eigenmodes and which modes are residual modes so that you can distinguish between them.

When generating dynamic substructures (see Generating a Reduced Structural Damping Matrix for a Substructure), residual modes usually provide the most benefit if the loading patterns defined in each of the load cases match the loading patterns defined under the corresponding substructure load cases in the substructure generation step.

By default, if you activate residual modes, all the calculated eigenmodes and residual modes are used in subsequent mode-based procedures, unless

You choose to obtain a new set of eigenmodes and residual modes in a new frequency extraction step.
You choose to select a subset of the available eigenmodes and residual modes in the mode-based procedure (selection of modes is described in each of the mode-based analysis type sections).

Residual modes cannot be calculated if the cyclic symmetric modeling capability is used.

Requesting Residual Modes Computation in an Eigenvalue Extraction Analysis

You can activate residual modes computation in an eigenfrequency extraction procedure. Residual modes extraction is supported only for the Lanczos and AMS eigensolvers. The Lanczos and AMS eigensolvers support several methods to specify data (loads and their locations) defining residual modes. Table 2 indicates the eigensolver support for each of the methods.

Table 2. Eigensolver support for methods to request residual modes.
Method	Residual Mode Definition	Lanczos	AMS	Subspace
1	Load cases in eigenfrequency extraction procedure	Yes	Yes	No
2	Specifying degrees of freedom in eigenfrequency extraction procedure	Yes	Yes	No
3	Loads specified in mode-based procedures following eigenfrequency extraction	Yes	Yes	No
4	Static perturbation step preceding eigenfrequency extraction	Yes	No	No

Input File Usage

FREQUENCY, RESIDUAL MODES

Abaqus/CAE Usage

Step module: StepCreate: Frequency: Basic: Include residual modes

Requesting Residual Modes Computation Using the Lanczos Eigensolver

The Lanczos eigensolver offers several methods for defining residual modes. Methods 1 and 2 take precedence over Method 4, which takes precedence over Method 3. Therefore, if the frequency extraction step contains load cases that define residual modes or specified degrees of freedoms for residual vectors, the preceding static perturbation step (as well as subsequent linear dynamics procedures) have no effect on the computed residual modes. Similarly, if a static perturbation step is defined prior to the frequency extraction procedure and the frequency extraction step contains no load cases or specified degrees of freedom for residual vectors, Abaqus/Standard defines the residual modes by the loads only from the static perturbation step.

Method 1 (Lanczos): Load Cases in Eigenfrequency Extraction

You can specify residual modes using the loads defined in the load cases in the eigenfrequency extraction step. For each load case, Abaqus/Standard calculates two residual modes: one to include the effects of all in-phase (real) loads and another to include the effects of all out-of-phase (imaginary) loads. If you specify only real or only imaginary loads in the load case, Abaqus/Standard calculates a single residual mode. There are no fundamental restrictions for the loads used in the load cases. Abaqus/Standard supports all loads allowed in the modal analysis steps (the steady-state dynamic and transient modal dynamic analysis procedures). Using this method, you cannot specify loads outside the load cases and boundary conditions within the load cases.

An example for Method 1 (Lanczos) is shown below.

STEP
FREQUENCY, EIGENSOLVER=LANCZOS, RESIDUAL MODES
…
LOAD CASE
CLOAD
DLOAD
END LOAD CASE
LOAD CASE
CLOAD
DLOAD
DSLOAD
END LOAD CASE
…
END STEP

Method 2 (Lanczos): Specifying Degrees of Freedom in Eigenfrequency Extraction

You can request additional residual modes by specifying degrees of freedom. For the Lanczos eigensolver, you can combine Method 2 with Method 1 or Method 3.

An example for Method 2 (Lanczos) is shown below.

STEP
FREQUENCY, EIGENSOLVER=LANCZOS, RESIDUAL MODES
first data line
(additional data lines specifying degrees of freedom for residual modes)
first node label, first DOF label
second node label, second DOF label
… (no load cases defined)
END STEP

Method 3 (Lanczos): Loads Specified in Mode-Based Procedures Following Eigenfrequency Extraction

If load cases are not specified in the eigenfrequency extraction step and there is no static perturbation step immediately preceding the eigenfrequency extraction step, Abaqus/Standard computes residual modes for loads applied in the subsequent mode-based procedure specified in the same analysis job (not in the restart analysis). Abaqus/Standard calculates one residual mode for all real loads and another for all imaginary loads (if they are allowed) for each load case. Otherwise, Abaqus/Standard assumes that all loads are part of a single load case and calculates only one real-imaginary residual mode pair for that particular step. Abaqus/Standard takes into account all loads specified in the subsequent mode-based procedure. However, it ignores amplitude curve definitions. Therefore, if you associate different loads within the same load case with different amplitude curves, Abaqus/Standard does not automatically create a residual mode per a group of loads sharing the same amplitude.

An example for Method 3 (Lanczos) is shown below.

(no preceding static perturbation step)
STEP
FREQUENCY, EIGENSOLVER=LANCZOS, RESIDUAL MODES
… (no load cases defined)
END STEP
STEP
STEADY STATE DYNAMICS
…
LOAD CASE
CLOAD
DLOAD
END LOAD CASE
LOAD CASE
CLOAD
DLOAD
DSLOAD
SLOAD
END LOAD CASE
END STEP

Method 4 (Lanczos): Static Perturbation Step Preceding Eigenfrequency Extraction

If you do not specify load cases in the eigenfrequency extraction step, you can define residual modes by specifying loads in a static perturbation step immediately preceding the eigenfrequency extraction step. If you specify multiple load cases in this static linear perturbation analysis, Abaqus/Standard calculates one residual mode for each load case; otherwise, it assumes that all loads belong to a single load case and calculates only one residual mode. When you request residual modes, the boundary conditions applied in the frequency extraction step must match those applied in the preceding static perturbation step. In addition, in the immediately preceding static perturbation step, Abaqus/Standard requires the following conditions:

If multiple load cases are used, the boundary conditions applied in each load case must be identical.
The boundary condition magnitudes are zero.

An example for Method 4 (Lanczos) is shown below.

STEP, PERTURBATION
STATIC
LOAD CASE
CLOAD
DLOAD
END LOAD CASE
LOAD CASE
CLOAD
DLOAD
DSLOAD
SLOAD
END LOAD CASE
END STEP
STEP
FREQUENCY, EIGENSOLVER=LANCZOS, RESIDUAL MODES
… (no load cases defined)
END STEP

Requesting Residual Modes Computation Using the AMS Eigensolver

The AMS eigensolver offers several methods for defining residual modes.

Method 1 (AMS): Load Cases in Eigenfrequency Extraction

Abaqus/Standard computes residual modes for the loads specified in the load cases in the eigenfrequency extraction step. It calculates one residual mode for each load case and for each loading type (real/imaginary). There are no fundamental restrictions for the loads used in the load cases. Abaqus/Standard supports all loads allowed in the modal analysis steps (the steady-state dynamic and transient modal dynamic analysis procedures). It takes the concentrated load magnitudes into account; therefore, each load case can specify loads combined from several differently scaled concentrated loads.

An example for Method 1 (AMS) is shown below.

STEP
FREQUENCY, EIGENSOLVER=AMS, RESIDUAL MODES
…
LOAD CASE
CLOAD
CLOAD
DLOAD
END LOAD CASE
LOAD CASE
CLOAD
CLOAD
CLOAD
DSLOAD
END LOAD CASE
…
END STEP

Method 2 (AMS): Specifying Degrees of Freedom in Eigenfrequency Extraction

You can request additional residual modes by specifying degrees of freedom. For the AMS eigensolver, you can combine Method 2 with Method 1 or Method 3.

An example for Method 2 (AMS) is shown below.

STEP
FREQUENCY, EIGENSOLVER=AMS, RESIDUAL MODES
first data line
(additional data lines specifying degrees of freedom for residual modes)
first node label, first DOF label
second node label, second DOF label
… (no load cases defined)
END STEP

Method 3 (AMS): Loads Specified in Mode-Based Procedures Following Eigenfrequency Extraction

If you do not specify load cases in the frequency extraction step, Abaqus/Standard computes residual modes for all degrees of freedom at which concentrated loads are applied in the subsequent mode-based procedures specified in the same analysis job (not in the restart analysis). It computes a residual mode for every degree of freedom loaded with the concentrated load.

An example for Method 3 (AMS) is shown below.

STEP
FREQUENCY, EIGENSOLVER=AMS, RESIDUAL MODES
… (no load cases defined)
END STEP
STEP
STEADY STATE DYNAMICS
…
LOAD CASE
CLOAD
DLOAD
END LOAD CASE
LOAD CASE
CLOAD
DLOAD
DSLOAD
END LOAD CASE
END STEP
STEP
MODAL DYNAMIC
CLOAD
DLOAD
END STEP

Evaluating Frequency-Dependent Material Properties

When frequency-dependent material properties are specified, Abaqus/Standard offers the option of choosing the frequency at which these properties are evaluated for use in the frequency extraction procedure. This evaluation is required because the stiffness cannot be modified during the eigenvalue extraction procedure. If you do not choose the frequency, Abaqus/Standard evaluates the stiffness associated with frequency-dependent springs and dashpots at zero frequency and does not consider the stiffness contributions from frequency domain viscoelasticity. If you do specify a frequency, only the real part of the stiffness contributions from frequency domain viscoelasticity is considered.

Evaluating the properties at a specified frequency is particularly useful in analyses in which the eigenfrequency extraction step is followed by a subspace projection steady-state dynamic step (see Subspace-Based Steady-State Dynamic Analysis). In these analyses the eigenmodes extracted in the frequency extraction step are used as global basis functions to compute the steady-state dynamic response of a system subjected to harmonic excitation at a number of output frequencies. The accuracy of the results in the subspace projection steady-state dynamic step is improved if you choose to evaluate the material properties at a frequency in the vicinity of the center of the range spanned by the frequencies specified for the steady-state dynamic step.

Input File Usage

FREQUENCY, PROPERTY EVALUATION=frequency

Abaqus/CAE Usage

Step module: StepCreate: Frequency: Other: Evaluate dependent properties at frequency

Generating a Flexible Body

Abaqus/Standard can generate a flexible body from a natural frequency extraction for use in the Simpack flexible body dynamics solver. Only the .sim file results format is supported. Simpack converts all of the data and units into a Flexible Body Interface (FBI) file.

A flexible body in Simpack can be kinematically connected to other bodies of the multibody system by joints or connections that constrain the flexible body in certain degrees of freedom. You must use a boundary condition in the natural frequency extraction to constrain those degrees of freedom.

You can match the range of extracted frequencies to the use case in the flexible body dynamics simulation.

Input File Usage

FLEXIBLE BODY, TYPE=SIMPACK

Abaqus/CAE Usage

Flexible body generation is not supported in Abaqus/CAE.

Initial Conditions

If the frequency extraction procedure is the first step in an analysis, the initial conditions form the base state for the procedure (except for initial stresses, which cannot be included in the frequency extraction if it is the first step). Otherwise, the base state is the current state of the model at the end of the last general analysis step (General and Perturbation Procedures). Initial stress stiffness effects (specified either through defining initial stresses or through loading in a general analysis step) are included in the eigenvalue extraction only if geometric nonlinearity is considered in a general analysis procedure before the frequency extraction procedure.

If initial stresses must be included in the frequency extraction and there is not a general nonlinear step before the frequency extraction step, a “dummy” static step—which includes geometric nonlinearity and which maintains the initial stresses with appropriate boundary conditions and loads—must be included before the frequency extraction step.

Initial Conditions describes all of the available initial conditions.

Boundary Conditions

Nonzero magnitudes of boundary conditions in a frequency extraction step are ignored; the degrees of freedom specified are fixed (Boundary Conditions).

Boundary conditions defined in a frequency extraction step are not used in subsequent general analysis steps (unless they are respecified).

In a frequency extraction step involving piezoelectric elements, the electric potential degree of freedom must be constrained at least at one node to remove numerical singularities arising from the dielectric part of the element operator.

Defining Primary and Secondary Bases for Modal Superposition Procedures

If displacements or rotations are to be prescribed in subsequent dynamic modal superposition procedures, boundary conditions must be applied in the frequency extraction step; these degrees of freedom are grouped into “bases.” The bases are then used for prescribing motion in the modal superposition procedure—see Transient Modal Dynamic Analysis.

Boundary conditions defined in the frequency extraction step supersede boundary conditions defined in previous steps. Hence, degrees of freedom that were fixed before the frequency extraction step are associated with a specific base if they are redefined with reference to such a base in the frequency extraction step.

The Primary Base

By default, all degrees of freedom listed for a boundary condition are assigned to an unnamed “primary” base. If the same motion is prescribed at all fixed points, the boundary condition is defined only once; and all prescribed degrees of freedom belong to the primary base.

Unless removed in the frequency extraction step, boundary conditions from the last general analysis step become fixed boundary conditions for the frequency step and belong to the primary base.

If all rigid body motions are not suppressed by the boundary conditions that make up the primary base, you must apply a suitable frequency shift to avoid numerical problems.

Input File Usage

BOUNDARY

The BOUNDARY option without the BASE NAME parameter can appear only once in a frequency extraction step.

Abaqus/CAE Usage

Load module: Create Boundary Condition

Secondary Bases

If the modal superposition procedure has more than one independent base motion, the driven nodes must be grouped together into “secondary” bases in addition to the primary base. The secondary bases must be named. (See Base motions in modal-based procedures.) Secondary bases are used only in modal dynamic and steady-state dynamic (not direct) procedures.

The degrees of freedom associated with secondary bases are not suppressed; instead, a “big” mass is added to each of them. To provide six digits of numerical accuracy, Abaqus/Standard sets each “big” mass equal to 10⁶ times the total mass of the structure and each “big” rotary inertia equal to 10⁶ times the total moment of inertia of the structure. Hence, an artificial low frequency mode is introduced for every degree of freedom in a secondary base. To keep the requested range of frequencies unchanged, Abaqus/Standard automatically increases the number of eigenvalues extracted. Consequently, the cost of the eigenvalue extraction step increases as more degrees of freedom are included in the secondary bases. To reduce the analysis cost, keep the number of degrees of freedom associated with secondary bases to a minimum. This can sometimes be done by reducing several secondary bases that all have the same prescribed motion to a single node by using BEAM type MPCs (General Multi-Point Constraints).

For the Lanczos and subspace iteration methods a negative shift must be used with either the rigid body modes or secondary bases.

The “big” masses are not included in the model statistics, and the total mass of the structure and the printed messages about masses and inertia for the entire model are not affected. However, the presence of the masses is noticeable in the output tables printed for the eigenvalue extraction step, as well as in the information for the generalized masses and effective masses. See Double cantilever subjected to multiple base motions for an example of the use of the base motion feature.

More than one secondary base can be defined by repeating the boundary condition definition and assigning different base names.

Input File Usage

BOUNDARY, BASE NAME=name

Abaqus/CAE Usage

Load module; Create Boundary Condition; Step: frequency_step; Category: Mechanical; Types for Selected Step: Secondary base; Constrained degrees-of-freedom: Region: select region, U1, U2, U3, UR1, UR2, and/or UR3

Controlling Damping for Low Frequency Modes

You can control damping of the low frequency modes (rigid body modes and low frequency modes with secondary base motions) in transient modal analyses. For more information, see Controlling Damping.

Loads

Applied loads (About Loads) are ignored during a frequency extraction analysis. If loads were applied in a previous general analysis step and geometric nonlinearity was considered for that prior step, the load stiffness determined at the end of the previous general analysis step is included in the eigenvalue extraction (General and Perturbation Procedures).

Predefined Fields

Predefined fields cannot be prescribed during natural frequency extraction.

Material Options

The density of the material must be defined (Density). The following material properties are not active during a frequency extraction: plasticity and other inelastic effects, rate-dependent material properties, thermal properties, mass diffusion properties, electrical properties (although piezoelectric materials are active), and pore fluid flow properties—see General and Perturbation Procedures.

Elements

Other than generalized axisymmetric elements with twist, any of the stress/displacement or acoustic elements in Abaqus/Standard (including those with temperature, pressure, or electrical degrees of freedom) can be used in a frequency extraction procedure.

Output

The eigenvalues (EIGVAL), eigenfrequencies in cycles/time (EIGFREQ), generalized masses (GM), composite modal damping factors (CD), participation factors for displacement degrees of freedom 1–6 (PF1–PF6) and acoustic pressure (PF7), and modal effective masses for displacement degrees of freedom 1–6 (EM1–EM6) and acoustic pressure (EM7) are written automatically to the output database as history data. Output variables such as stress, strain, and displacement (which represent mode shapes) are also available for each eigenvalue; these quantities are perturbation values and represent mode shapes, not absolute values.

The eigenvalues and corresponding frequencies (in both radians/time and cycles/time) are also listed automatically in the printed output file, along with the generalized masses, composite modal damping factors, participation factors, and modal effective masses.

The AMS eigensolver does not compute composite modal damping factors or modal effective masses. In addition, you cannot request output to the results (.fil) file.

You can restrict output to the results, data, and output database files by selecting the modes for which output is desired (see Output to the Data and Results Files and Output to the Output Database).

Input File Usage

Use one of the following options:

EL FILE, MODE, LAST MODE
EL PRINT, MODE, LAST MODE
OUTPUT, MODE LIST

Abaqus/CAE Usage

Step module: OutputField Output RequestsCreate: Frequency: Specify modes

Energy Output

Several types of energy output variables are supported in eigenvalue extraction procedures. They include the elastic strain energy density (SENER), whole element variables (ELKE and ELSE), whole element energy density variables (EKEDEN and ESEDEN), and whole and partial model variables (ALLKE and ALLSE). The values of all of these energy variables, except SENER, are normalized. Normalization is performed for each eigenmode separately, such that the kinetic and strain energies add up to one for the whole model. Computation of the energy variables is implemented for all but residual and singular acoustic modes.

The energy variables that can be written to the output database are defined in Total Energy Output Quantities.

Input File Usage

ENERGY OUTPUT
list of output variables

Abaqus/CAE Usage

Step module: history output request editor: Select from list below

Input File Template

HEADING
…
BOUNDARY
Data lines to specify zero-valued boundary conditions
INITIAL CONDITIONS
Data lines to specify initial conditions
**
STEP (,NLGEOM)
If NLGEOM is used, initial stress and preload stiffness effects
are included in the frequency extraction step
STATIC
…
CLOAD and/or DLOAD
Data lines to specify loads
TEMPERATURE and/or FIELD
Data lines to specify values of predefined fields
BOUNDARY
Data lines to specify zero-valued or nonzero boundary conditions
END STEP
**
STEP, PERTURBATION
STATIC
…
LOAD CASE, NAME=load case name
Keywords and data lines to define loading  for this load case
END LOAD CASE
…
END STEP
**
STEP
FREQUENCY, EIGENSOLVER=LANCZOS, RESIDUAL MODES
Data line to control eigenvalue extraction
BOUNDARY

BOUNDARY, BASE NAME=name
Data lines to assign degrees of freedom to a secondary base
END STEP