# Frequency Response Analysis

Calculates the response of a structure to steady-state oscillatory excitation.

Typical applications are noise, vibration and harshness (NVH) analysis of vehicles, rotating machinery, transmissions, and powertrain systems.

Frequency response analysis is used 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 of given 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 $\mathrm{\Omega}$.

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.

## Direct Frequency Response Analysis

Direct frequency response analysis can be used to compute the structural responses directly at discrete excitation frequencies $\mathrm{\Omega}$ by solving a set of complex matrix equations.

- $M$
- Mass matrix
- $C$
- Damping matrix
- $K$
- Stiffness matrix
- $u$
- Displacement vector
- $f$
- Load vector

- Using a uniform structural damping coefficient $$G$$.
- Structural element damping is defined using the damping coefficient, $$GE$$ on the material entries, as well as $$GE$$ on bushing and spring element property definitions. These form the matrix $${C}_{GE}$$.
- Viscous damping is generated by damper elements. These form the matrix $${C}_{1}$$.

The equation of motion is solved directly using complex algebra.

### Run Direct Frequency Response Analysis

The Loads and Boundary Conditions are defined in the Bulk Data Entry section of the input deck. They need to be referenced in the Subcase Information section using an SPC and DLOAD statement in a SUBCASE.

OptiStruct does not support inertia relief for direct frequency response analysis. The solver 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`.

## Modal Frequency Response Analysis

The modal method first performs a normal modes analysis to obtain the eigenvalues $${\lambda}_{i}$$ and the corresponding eigenvectors $$A$$ of the system.

The modal mass matrix ${A}^{\text{T}}MA$ and the modal stiffness matrix ${\text{A}}^{T}KA$ 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.

Here, the matrices $${A}^{\text{T}}{C}_{GE}A$$ and $${A}^{\text{T}}{C}_{1}A$$ are generally non-diagonal. Then the coupled problem is similar to the system solved in the direct method, however 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 ${g}_{i}$ versus natural frequency ${f}_{i}^{freq}$. If this approach is used, no structural element or viscous damping should be defined.

- $${\zeta}_{i}={c}_{i}/\left(2{m}_{i}{\omega}_{i}\right)$$
- Modal damping ratio.
- ${\omega}_{i}^{2}$
- Modal eigenvalue.

- $$G$$
- Structural damping.
- $$CRIT$$
- Critical damping.
- $$Q$$
- Quality factor.

`KDAMP`, -1 is used. Then the uncoupled equation becomes:

A METHOD statement is required for the modal method to control the normal modes analysis. The METHOD statement can refer to either EIGRL or EIGRA Bulk Data Entry.

### Residual Vector Generation (Increases accuracy)

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.

- 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. This is the default method since it is generally more accurate.
- 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.

### Modal Frequency Response Analysis with Enforced Motion

- Relative Method:
In this case, the solution proceeds in two stages. First, a static analysis with the enforced motion is solved to obtain the static displacements. Then, the dynamic analysis is solved using the previously calculated static displacements and the eigenvectors. This method is relatively less efficient, but leads to more accurate solutions and is the default method.

- Total/Absolute Method:
In this case, the solution proceeds in a single stage and the calculation of static displacements is not needed. The contribution of modal dynamic load would directly come from applied displacement/velocity/acceleration at the SPCD degrees of freedom. This method is computationally efficient as it avoids calculation of static displacement vectors.

Refer to PARAM, ENFMETH to control the calculations with these methods.

### Run Modal Frequency Response Analysis

#### Input

The Loads and Boundary Conditions are defined in the Bulk Data Entry section of the input deck. They need to be referenced in the Subcase Information section using an SPC and DLOAD statement in a SUBCASE.

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.

Frequency-dependent materials (MATFi Bulk Data Entries) can be used in Direct and Modal Frequency Response Analysis, via TABLEDi entries for corresponding fields on the MATi entries. MATF1, MATF2, MATF3, MATF8, MATF9 and MATF10 Bulk Data Entries can be used to define the currently available frequency-dependent materials.

Frequency-dependent properties (PBUSHT Bulk Data Entry) can also be used in Frequency Response Analysis, via TABLEDi entries for the corresponding fields on the PBUSHT entry.

#### Default Solver for Modal FRF Solution

The standard internal solver is used by default for Modal Frequency Response Analysis. However, for some classes for models, improved performance may be obtained by using the Faster Modal Solution Method (FASTFR) or the Fast Frequency Response Solver (FastFRS).

#### Residual Vectors

Residual vectors are relevant for modal FRF/acoustics/transient analysis. They enhance the accuracy of these analyses and, hence, are computed by default. You can control RESVEC calculations using the case control statement:

RESVEC(APPLOD/UNITLOD,DAMPLOD/NODAMP)=Value

Where, Value can be Yes or No. The keyword(s) within parentheses are ignored, if the Value specified is No - all RESVEC calculations are turned off. The keyword APPLOD generates RESVECs based on the dynamic loading of the modal FRF/acoustics/transient analysis. The keyword UNITLOD generates RESVECs based on unit loads at the dynamic loading's degrees of freedom. The keyword DAMPLOD generates viscous damping RESVECs based on unit loads at the viscous damping degrees of freedom. The keyword NODAMP turns off the generation of the viscous damping RESVECs that are otherwise generated by default. Even though DAMPLOD and NODAMP are options in the case control, they are global switches that will be applied to all the modal FRF/acoustics/transient subcases in the model.

When the underlying eigenvalue analysis is done using the Lanczos method, the default RESVECs are generated based on the applied loading and viscous damping degrees of freedom. If the underlying eigenvalue analysis is done using AMSES or AMLS, the default RESVECs are generated based on unit loading at the load degrees of freedom and viscous damping degrees of freedom. Residual vectors are always generated if enforced displacements, velocities or accelerations are defined. In addition, if there is USET U6 data, residual vectors will be calculated if the AMSES or AMLS eigensolver is used. USET U6 residual vectors will not be calculated if the Lanczos eigensolver is used.

When residual vectors are included, Inertia Relief will be
applied by default to unconstrained models. If inertia relief is not desired for
RESVECs, it has to be turned off using
PARAM, `INREL`, 0.

When residual vectors are included, the eigenmodes from the underlying eigenvalue
analysis of the FRF/transient subcase are used in inertia relief. All modes with
eigenvalues below a limit value (`FZERO`) are used as rigid body
modes in the inertia relief analysis. If there are no eigenmodes below
`FZERO`, up to 6 global rigid body modes are internally
generated based on the geometry of the model and used in the inertia relief. You can
set `FZERO` using PARAM,
`FZERO`, Value. The default value for
`FZERO` is 0.1.

## Output

The results of a frequency response analysis are displacements, velocities, accelerations, forces, stresses, and strains. The usual output entries like STRESS, STRAIN, DISPLACEMENT, etc. can be used to request corresponding output values.

DISP(MODAL) can be used to output only the eigenvectors in Modal FRF/Transient response. DISP(MODAL,NODAL) can be used to output both the eigenvectors and the corresponding FRF/Transient response results.

KDYN can be used to output dynamic stiffness in Direct and Modal Frequency response analysis.

PARAM,
`ENFMOTN`, REL can be used to generate
displacement, velocity and acceleration output relative to the specified enforced
motion. In such cases, subsequently calculated outputs like stresses and forces are
also generated relative to the specified enforced motion. PARAM,
`ENFMOTN`, TOTAL/ABS can be
used to generate the total output values including the specified enforced motion
(TOTAL/ABS is the default).