.Frequency response analysis is used to calculate the response of a structure about steady state oscillatory excitation. Typical applications are noise, vibration and harshness analysis of vehicles, rotating machinery, and transmissions.
The analysis is to compute the response of the structure, which is actually transient, in a static frequency domain. The loading is sinusoidal. A simple case is a load that has an amplitude at a specified frequency. The response occurs at the same frequency, and damping would lead to a phase shift (Figure 1).
The loads can be forces, displacements, velocity, and acceleration.
They are dependent on the excitation frequency .
The results from a frequency response analysis are displacements, velocities, accelerations, forces, stresses, and strains. The responses are usually complex numbers that are either given as magnitude and phase angle or as real and imaginary part.
The direct and modal frequency response are implemented in OptiStruct.
Figure 1: Excitation and response of a frequency response analysis.
The direct frequency response analysis computes the structural
responses directly at discrete excitation frequencies by
solving a set of complex matrix equations.
The quantity 
is the loading angular frequency.
The harmonic motion assumes a harmonic response.
The vector u is the displacement vector. Then, a complex matrix for dynamic analysis can be derived that has the following real and imaginary parts:
The matrix K is the stiffness matrix, the matrix M the mass matrix.
There are three ways to define damping in the system.
Using a uniform structural damping coefficient G.
Structural element damping using
the damping coefficients GE on
the materials as well as GE on
bushing and spring element property definitions. These form the matrix
.
Viscous damping formed by the
damper elements. These form the matrix 
.
The equation of motion is solved directly using complex algebra.
The frequency response loads and boundary conditions are defined in the bulk data section of the input deck. They need to be referenced in the subcase information section using an SPC and DLOAD statement in a SUBCASE.
Inertia relief is not implemented for direct frequency response in OptiStruct. OptiStruct will error out if it is attempted.
A frequency set must be referenced using a FREQUENCY statement.
In addition to the various damping elements and material damping, uniform structural damping G can be applied using PARAM, G.
The modal method first performs a normal modes analysis to
obtain the eigenvalues 
and the corresponding eigenvectors
of the system. The response can be expressed as a scalar
product of the eigenvectors X
and the modal responses d.
The equation of motion without damping is then transformed into modal coordinates using the eigenvectors.
The modal mass matrix 
and the modal stiffness
matrix 
are diagonal. If the eigenvectors are normalized
with respect to the mass matrix, the modal mass matrix is the unity matrix
and the modal stiffness matrix is a diagonal matrix holding the eigenvalues
of the system. This way, the system equation is reduced to a set of uncoupled
equations for the components of d
that can be solved easily.
The inclusion of damping, as discussed in the direct method, yields:
Here, the matrices 
and 
are
generally non-diagonal. The then coupled problem is similar to the system
solved in the direct method, but of much lesser degree of freedom. It
is solved using the direct method.
The evaluation of the equation of motion is much faster if
the equations can be kept decoupled. This can be achieved if the damping
is applied to each mode separately. This is done through a damping table
TABDMP1 that lists damping values 
versus natural frequency 
. If this approach
is used, no structural element or viscous damping should be defined.
The decoupled equation is
where 
is the modal damping ratio, and 
is the modal eigenvalue.
Three types of modal damping values 
can be
defined: G – Structural damping, CRIT – Critical damping, and Q – Quality
factor. They are related through the following three equations at resonance:
Modal damping is entered in to the complex stiffness matrix as structural damping if PARAM, KDAMP, -1 is used. The then uncoupled equation becomes:
The accuracy of the modal method can be vastly improved by adding the displacement vectors of a static analysis based on the dynamic loading to the matrix of eigenvectors X. These vectors are frequently referred to as residual vectors, the method as the modal acceleration.
There are two ways this is implemented in OptiStruct. The unit load method generates residual vectors based on static loads which are unit vectors at the dynamic load degrees of freedom. That is, the static loads for the residual vector generation are unit vectors at the degrees of freedom where the dynamic load is applied. The number of residual vectors is equal to the number of loaded degrees of freedom. The applied load method generates a maximum of two residual vectors which are the dynamic load vector at a loading frequency of zero. If the real and the imaginary parts of the dynamic load are the same, or if one of them is zero, only one of them is used. This is the default method since it is generally more efficient.
In the case of excited displacements, the residual vectors are obtained by solving static load cases with unit displacements at the same degrees of freedom as the dynamic excited displacement degrees of freedom.
The following image illustrates the effect that the use of the residual vectors has on the result accuracy of the modal frequency response analysis (FRA) compared to the accurate direct method.
The frequency response loads and boundary conditions are defined in the bulk data section of the input deck. They need to be referenced in the subcase information section using an SPC and DLOAD statement in a SUBCASE.
Residual vectors can be activated using the subcase statement RESVEC with the options APPLOD or UNITLOD. They are computed by default. Residual vectors are always generated if enforced displacements, velocities or accelerations are defined.
When residual vectors are included, inertia relief can be applied to unconstrained models. A SUPORT1 subcase entry references the boundary conditions that restrain the rigid body motions. These restraints can also be defined without subcase reference using the SUPORT bulk data entry or automated using PARAM, INREL, -2.
A frequency set must be referenced using a FREQUENCY statement. A METHOD statement is required for the modal method to control the normal modes analysis. In order to save computational effort, previously saved eigenvectors can be retrieved using the EIGVRETRIEVE subcase statement.
In addition to the various damping elements and material damping, uniform structural damping G can be applied using PARAM, G.
Modal damping is being applied using the SDAMPING reference of a damping table TABDMP1. The parameter PARAM, KDAMP is to define the method of applying the damping table.