Solvers Overview: Natural Frequency

Description

The Natural Frequency solver is used to calculate the natural frequencies (or free vibration frequencies) and corresponding vibration modes of an undamped structure. The natural frequency analysis problem is formulated as the following eigenvalue problem:

where

= global stiffness matrix,

= Global mass matrix,

= Circular frequency (radians/sec), natural frequency (Hertz), and

= Vibration mode (shape) vector.

Initial conditions may be considered by the Natural Frequency solver to include the effects of stress stiffening, contact status and so on. When stress stiffening effects are included, a slightly different eigenvalue problem is solved, namely

where is the geometric, or stress, stiffness matrix corresponding to the results of the load case used as initial conditions.

Procedure

The Natural Frequency solver executes the following steps:

Calculates and assembles the element stiffness and mass matrices to form the global stiffness and mass matrices. In the stiffness calculation, material temperature dependency is considered through the user nominated temperature case (see Special Topics: Temperature Dependence). Either a consistent or lumped mass matrix can be used according to the solver option setting (see Entities: Consistent vs Lumped Mass). Constraints and links are assembled in this process, however, the constant terms for enforced displacements, shrink links and multi-point links are ignored, and the restraints are treated as fixed restraints.
If an initial file has been selected to define the initial stress state of the structure, a geometric stiffness matrix may be formed and assembled into the global stiffness matrix to account for stress stiffening/softening effects on natural frequencies. The geometric stiffness matrix is always added when the initial file comes from a linear static analysis, and when the initial file comes from a nonlinear static or quasi-static analysis executed with the GNL option. For initial files from nonlinear static and quasi-static analysis without the GNL option, the geometric stiffness matrix can be included on request.

If material nonlinearity, point contacts, cutoff bars or compression-only supports are considered in the initial solution, a tangent stiffness matrix will be assembled for the natural frequency analysis based on the state of these nonlinear effects in the selected result case.

If the initial file considered nonlinear geometry, the deformed geometry will be used as the initial shape of the structure in the natural frequency analysis - vibration is assumed to be centred on this deformed shape. See Special Topics: Solution Restart.
Modifies the stiffness matrix if a shift value is applied.
Solves the eigenvalue problem to calculate natural frequencies and the corresponding mode shapes using the Sub-Space Iteration method.

Notes

To help the user visualise the results, stress and strain patterns may be generated, although these are not quantitatively meaningful.
Frequency shift can be used to calculate higher modes by excluding lower modes. A special application of the shift is in the analysis of unconstrained structures. If the solver detects rigid body motion, a shift of -1.0 Hz may be automatically applied (if requested by the user, see SOLVERS Parameters: EIGENVALUE) and a message is given. If the shift is appropriate, one or more rigid body modes will be calculated, in addition to deformational modes, depending on the number of modes requested by the user.
The Sturm Sequence check is an effective way to check the convergence of the sub-space iteration method to ensure that the eigenvalue solution has converged and no eigenvalues are missed.
When the mode participation factors are requested, the engineering modal mass and engineering modal stiffness are also given. See Results Options: Displacement Tab.
By defining a material damping coefficient and participation direction vector, an effective damping coefficient, modal participation factors and modal mass participation ratios can be calculated for each mode. The calculated damping coefficients can be used in further dynamic analysis in the SOLVERS: Spectral Response Settings, SOLVERS: Harmonic Response Settings and SOLVERS: Linear Transient Dynamic Settings solvers.

The modal mass participation ratios are calculated using the following equation:

and the modal participation factors are calculated using the following equation:

where

= global mass matrix,

= global displacement vector, determined by the excitation direction, and

= mode shape vector of the ^th mode.

The effective damping coefficients for each mode are calculated by the following equation:

where

= number of elements,

= global stiffness matrix,

= stiffness matrix of element expanded into the global stiffness matrix,

= mode shape vector for mode ,

= damping ratio of element , and

= effective modal damping ratio for mode .