Products: ABAQUS/Standard ABAQUS/CAE
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;
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 6.1.2);
can include friction, damping, and unsymmetric load stiffness contributions; and
cannot be used in a model defined as a cyclic symmetric structure (“Analysis of models that exhibit cyclic symmetry,” Section 7.8.3).
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 complex eigenvector (the mode of vibration); and
and 
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 |
You can specify a positive or negative shift point, 
, 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 , , , |
| ABAQUS/CAE Usage: | Step module: Create Step: Linear perturbation: Complex frequency: Frequency shift (cycles/time): |
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. |
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 |
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 19.4.1) 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).
The density of the material must be defined (see “Density,” Section 9.2.1). 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.
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.
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.
*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