6.3.6 Complex eigenvalue extraction
Products: Abaqus/Standard Abaqus/CAE
References
Overview
The complex eigenvalue extraction procedure:
performs eigenvalue extraction to calculate the complex eigenvalues and the corresponding complex mode shapes of a system;
is a linear perturbation procedure;
requires that an eigenfrequency extraction procedure (“Natural frequency extraction,” Section 6.3.5) be performed prior to the complex eigenvalue extraction;
can use the high-performance SIM software architecture (see “Using the SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1);
will include initial stress and load stiffness effects due to preloads and initial conditions if nonlinear geometric effects are included in the base state step definition (“General and linear perturbation procedures,” Section 6.1.3);
can include friction, damping, and unsymmetric load stiffness contributions;
can include unsymmetric damping and stiffness contributions in acoustic finite elements due to underlying mean flow (“Acoustic, shock, and coupled acoustic-structural analysis,” Section 6.10.1); and
cannot be used in a model defined as a cyclic symmetric structure (“Analysis of models that exhibit cyclic symmetry,” Section 10.4.3).
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:
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 right complex eigenvector;
is the left complex eigenvector and is defined as follows:
is a transpose conjugate left eigenvectorM 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 “Defining an analysis,” Section 6.1.2).
| 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 shift point, S, in cycles per time, for the complex eigenvalue extraction procedure (S ≥ 0). Abaqus/Standard reports the complex eigenmodes, 
, in order of increasing 
so that the modes with the imaginary part closest to a given shift point are 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 |
Normalization
For complex eigenvalue extraction analysis both displacement and modal complex eigenvector normalization are available. Displacement normalization is the default in SIM-based analysis. Modal normalization is the only option available if the SIM-based architecture is not used.
If displacement normalization is selected, the complex eigenvectors are normalized so that the largest value in each vector is unity and the imaginary part is zero. If modal normalization is selected, only the complex eigenvectors of the projected system (GU) are normalized using the displacement method and no normalization of the complex eigenvectors in the finite element subspace is performed. For large eigenproblems the displacement normalization can become time consuming; therefore, modal normalization is recommended.
| Input File Usage: | Use the following option to select displacement normalization (available only if the SIM-based architecture is used): |
*COMPLEX FREQUENCY, NORMALIZATION=DISPLACEMENT Use the following option to select modal normalization (the only option if the SIM-based architecture is not used): *COMPLEX FREQUENCY, NORMALIZATION=MODAL |
| Abaqus/CAE Usage: | You cannot select the normalization method of the complex eigenvectors in Abaqus/CAE; the default method is used. |
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 |
Right and left complex eigenvectors
For complex eigenvalue extraction analysis right or left complex eigenvectors can be requested. By default, the right eigenvectors are extracted. The left eigenvectors are available only in analyses that are based on the SIM architecture. You can extract both right and left complex eigenvectors in the same analysis, but they must be requested in separate steps. You should select modal normalization of the complex eigenvectors if you want to extract both the right and left eigenvectors.
| Input File Usage: | Use the following option to extract the right complex eigenvectors: |
*COMPLEX FREQUENCY, RIGHT EIGENVECTORS (default, the only option if the SIM architecture is not used) Use the following option to extract the left complex eigenvectors: *COMPLEX FREQUENCY, LEFT EIGENVECTORS (only if the SIM architecture is used) |
| Abaqus/CAE Usage: | Only the right complex eigenvectors are extracted in Abaqus/CAE. |
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 nodes in contact the tangential degrees of freedom will be constrained.
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 Guide. 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 32.2.1), by “Rayleigh” damping associated with materials and elements (see “Material damping,” Section 26.1.1), 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, damping contributions from frequency-domain viscoelasticity, and all types of modal damping (except composite modal damping) are supported in complex eigenvalue extraction using the high-performance SIM architecture.
Prescribing motion, transport velocity, and acoustic flow velocity
Motion, transport velocity, and acoustic flow velocity affect complex frequency analyses. Motion and transport velocity must be specified in a preceding steady-state transport general step, and their effects are included in the complex frequency step. The acoustic flow velocity has no effect in steady-state transport steps, and acoustic flow velocities specified in a steady-state transport step are not propagated to perturbation steps. The acoustic flow velocity must be specified in each linear perturbation step where it is desired.
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.
Loads
Applied loads (“Applying loads: overview,” Section 34.4.1) 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 6.1.3).
Coriolis distributed loading adds an unsymmetric contribution to the damping operator, which is currently accounted for only in solid and truss elements.
Material options
The density of the material must be defined (see “Density,” Section 21.2.1). 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 effective 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 restrict output to the data file and output database file by selecting the modes for which output is desired (see “Output to the data and results files,” Section 4.1.2) or “Output to the output database,” Section 4.1.3). Output to the results (.fil) file is not available for the complex eigenvalue extraction procedure.
Setting the cutoff value for complex eigenmodes
You can also set the cutoff value for complex eigenmodes, so only complex modes with the real part of the eigenvalue higher than the cutoff value are written to the output database file. The default cutoff value is 0.0. If the cutoff value is not set, all complex modes are output.
| Input File Usage: | Use one of the following options to select complex eigenmodes for output: |
*COMPLEX FREQUENCY, UNSTABLE MODES ONLY *COMPLEX FREQUENCY, UNSTABLE MODES ONLY=value |
The SIM architecture
The complex eigenvalue extraction analysis can be performed using the SIM architecture. The advantages of performing the complex eigenvalue extraction procedure using the SIM architecture are as follows:
structural damping, including damping defined with viscoelastic material, is taken into account;
modal damping can be specified;
matrices representing the stiffness, mass, and damping can be defined (both symmetric and unsymmetric matrices are supported); and
the AMS eigensolver can be used to generate the projection subspace for the complex eigenvalue extraction.
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 … *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(,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