### 6.3.6 Complex eigenvalue extraction

Products: ABAQUS/Standard  ABAQUS/CAE

### Overview

The complex eigenvalue extraction procedure:

### Complex eigenvalue extraction

The complex eigenvalue extraction procedure uses a projection method to extract the complex eigenvalues of the current system. The eigenvalue problem of the finite element model is formulated in the following manner:

where

is the mass matrix (which is symmetric and, in general, is semi-positive definite);

is the damping matrix;

is the stiffness matrix (which can include initial stress stiffness and friction effects and, therefore, in general is unsymmetric);

is the complex eigenvalue;

is the complex eigenvector (the mode of vibration); and

M and N

are degrees of freedom.

The complex eigenvalue extraction procedure in ABAQUS/Standard uses a subspace projection method; thus, the eigenmodes of the undamped system with the symmetrized stiffness matrix must be extracted using the eigenfrequency extraction procedure prior to the complex eigenvalue extraction step. By default, the entire subspace is used as the base vector; this subspace can be reduced as described below. ABAQUS/Standard always computes all the complex eigenmodes available in the projection subspace (taking into account any user-specified modifications to the subspace). The user-specified number of requested eigenmodes and frequency range for the complex eigenvalue extraction procedure do not influence the number of computed complex eigenmodes. It determines only the number of reported modes, which cannot be higher than the dimension of the projected subspace. To modify the number of computed eigenmodes, reduce the projection subspace as described below or change the number of eigenmodes extracted in the prior natural frequency extraction step accordingly. If you do not specify the number of requested complex modes or the frequency range, all the computed modes will be reported.

To take into account the unsymmetric effects, the unsymmetric matrix solution and storage scheme is used automatically for a complex eigenvalue extraction step. The unsymmetric effects will be disregarded if you specify that the symmetric solution and storage scheme should be used (see Procedures: overview, Section 6.1.1).

 Input File Usage: ```*COMPLEX FREQUENCY number of complex eigenmodes, frequency_min, frequency_max```

 ABAQUS/CAE Usage: Step module: Create Step: Linear perturbation: Complex frequency: Number of eigenvalues requested: All or Value, Minimum frequency of interest (cycles/time): value, Maximum frequency of interest (cycles/time): value

#### Shift point

You can specify a positive or negative shift point, S, in cycles per time, for the complex eigenvalue extraction procedure. ABAQUS/Standard will report the complex eigenmodes, , in order of increasing so that the modes with the imaginary part closest to a given shift point will be reported first. This feature is useful when a particular frequency range is of concern. The default is no shift.

 Input File Usage: ```*COMPLEX FREQUENCY , , , S```

 ABAQUS/CAE Usage: Step module: Create Step: Linear perturbation: Complex frequency: Frequency shift (cycles/time): S

#### Selecting the eigenmodes on which to project

You can select eigenmodes of the undamped system with the symmetrized stiffness matrix on which the subspace projection will be performed. You can select them by specifying the mode numbers individually, by requesting that ABAQUS/Standard generate the mode numbers automatically, or by requesting the eigenmodes that belong to specified frequency ranges. If you do not select the eigenmodes, all modes extracted in the prior eigenfrequency extraction step are used in the modal superposition.

 Input File Usage: Use one of the following options to select the eigenmodes by specifying mode numbers: ```*SELECT EIGENMODES, DEFINITION=MODE NUMBERS *SELECT EIGENMODES, GENERATE, DEFINITION=MODE NUMBERS```Use the following option to define the eigenmodes by specifying a frequency range:`*SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE`

 ABAQUS/CAE Usage: You cannot select the eigenmodes in ABAQUS/CAE; all modes extracted are used in the subspace projection.

#### 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 complex eigenvalue extraction procedure. This evaluation is necessary because the operators cannot be modified during the eigenvalue extraction procedure. If you do not choose the frequency, ABAQUS/Standard evaluates the stiffness and damping associated with frequency-dependent springs and dashpots at zero frequency and does not consider the stiffness and damping contributions from frequency-domain viscoelasticity. If you do specify a frequency, the stiffness and damping contributions from frequency-domain viscoelasticity are considered.

 Input File Usage: `*COMPLEX FREQUENCY, PROPERTY EVALUATION=frequency`

 ABAQUS/CAE Usage: Step module: Create Step: Complex Frequency: Other: Evaluate dependent properties at frequency: value

### Contact conditions with sliding friction

ABAQUS/Standard automatically detects the contact nodes that are slipping due to velocity differences imposed by the motion of the reference frame or the transport velocity in prior steps. At those nodes the tangential degrees of freedom will not be constrained and the effect of friction will result in an unsymmetric contribution to the stiffness matrix. At other contact nodes the tangential degrees of freedom will be constrained as in a regular linear perturbation analysis.

Friction at contact nodes at which a velocity differential is imposed can give rise to damping terms. There are two kinds of friction-induced damping effects. The first effect is caused by the friction forces stabilizing the vibrations in the direction perpendicular to the slip direction. This effect exists only in three-dimensional analysis. The second effect is caused by a velocity-dependent friction coefficient. If the friction coefficient decreases with velocity (which is usually the case), the effect is destabilizing and is also known as “negative damping.” For more details, see Coulomb friction, Section 5.2.3 of the ABAQUS Theory Manual. The complex eigensolver allows you to include these friction-induced contributions to the damping matrix.

 Input File Usage: `*COMPLEX FREQUENCY, FRICTION DAMPING=YES`

 ABAQUS/CAE Usage: Step module: Create Step: Linear perturbation: Complex frequency: Include friction-induced damping effects

### Damping

In complex eigenvalue extraction analysis damping can be defined by dashpots (see Dashpots, Section 26.2.1), by “Rayleigh” damping associated with materials and elements (see Material damping, Section 20.1.1), by viscoelasticity included in the material definitions (see Frequency domain viscoelasticity, Section 17.7.2), and by quiet boundaries on infinite elements or acoustic elements. In addition, as described in “Contact conditions with sliding friction” above, friction-induced damping can be included.

Structural damping and all types of modal damping are not supported in the complex eigenvalue extraction procedure.

### Prescribing motion, transport velocity, and acoustic flow velocity

The motion, transport velocity, and acoustic flow velocity options affect complex frequency analyses. The motion and transport velocity options must be specified in a preceding steady-state transport general step, and their effects are included in the complex frequency step. In general, acoustic flow velocity propagates like transport velocity. If it is used in a general step, such as steady-state transport, it propagates to subsequent steps unless it is changed in those steps. If it is not used in a general step, it should be used in each linear perturbation step where it is desired. It is good practice to use acoustic flow velocity in steady-state transport steps, even though it does nothing to the elements in those steps, to ensure that the rotating motions for the fluid and solid are consistent from general to perturbation steps.

### Initial conditions

Initial conditions cannot be specified for complex eigenvalue extraction.

### Boundary conditions

Boundary conditions cannot be defined during complex eigenvalue extraction. The boundary conditions will be the same as in the prior natural frequency extraction analysis.

Applied loads (Applying loads: overview, Section 27.4.1) are ignored during a complex eigenvalue extraction. If loads were applied in a previous general analysis step in which nonlinear geometric effects were included, the load stiffness determined at the end of the previous general analysis step is included in the complex eigenvalue extraction (see General and linear perturbation procedures, Section 6.1.2).

### Predefined fields

Predefined fields cannot be prescribed during complex eigenvalue extraction.

### Material options

The density of the material must be defined (see Density, Section 16.2.1). The following material properties are not active during complex eigenvalue extraction:

• plasticity and other inelastic effects;

• rate-dependent material properties, excluding friction, which can be rate dependent if the velocity differential on the contact interface exists;

• thermal properties;

• mass diffusion properties;

• electrical properties (although piezoelectric materials are active); and

• pore fluid flow properties.

### Elements

Other than generalized axisymmetric elements with twist, any of the stress/displacement elements in ABAQUS/Standard (including those with temperature or pressure degrees of freedom) can be used in complex eigenvalue extraction.

### Output

The real (EIGREAL) and imaginary (EIGIMAG) parts of the eigenvalues, ( and ); frequencies in cycles/time (EIGFREQ); and damping ratios (DAMPRATIO = ) are written automatically to the data (.dat) file and to the output database (.odb) file as history data. In addition, you can request that the generalized displacements (GU), which are the modes of the projected system, be written to the output database file (see Output to the output database, Section 4.1.3). 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 only energy density available in eigenvalue extraction procedures is the elastic strain energy density, SENER. All of the output variable identifiers are outlined in ABAQUS/Standard output variable identifiers, Section 4.2.1.

You can select the eigenmodes for which output to the data file (see Output to the data and results files, Section 4.1.2) or the output database file (see Output to the output database, Section 4.1.3) is desired. Output to the results (.fil) file is not available for the complex eigenvalue extraction procedure.

### Input file template

```*HEADING
…
*SURFACE INTERACTION
*FRICTION
Specify zero friction coefficient
*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
will be included in the eigenvalue extraction steps
*STATIC
…
*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(,NLGEOM)
*STATIC
Data line to define incrementation
*CHANGE FRICTION
*FRICTION
Data lines to redefine friction coefficient
*MOTION, ROTATION or TRANSLATION
Data lines to define the velocity differential
*END STEP
**
*STEP
*FREQUENCY
Data line to control eigenvalue extraction
*END STEP
**
*STEP
*COMPLEX FREQUENCY
Data line to control complex eigenvalue extraction
*SELECT EIGENMODES
Data lines to define applicable mode ranges
*END STEP```