# Linear Transient Analysis

Calculates the response of a structure to time-dependent loads. Typical applications are structures subject to earthquakes, wind, explosions, or a vehicle going through a pothole.

The loads are time-dependent forces and displacements. Initial conditions define the initial displacement and initial velocities in grid points.

The results of a transient response analysis are displacements, velocities, accelerations, forces, stresses, and strains. The responses are usually time-dependent.

The matrix $K$ is the global stiffness matrix, the matrix $M$ the mass matrix, and the matrix $C$ is the damping matrix formed by the damping elements. The initial conditions are part of the problem formulation and are applicable for the direct transient response only. The equation of motion is integrated over time using the Newmark beta method. A time step and an end time need to be defined.

Loading for transient analysis can be applied via the TLOADi entries.
The `EXCITEID` field on the TLOADi entry identifies
the type of loading which can be applied, including forces, enforced displacement,
enforced velocity, enforced acceleration, enforced temperature, enforced joule loss
density, and also external loading via
.rsp/.rpc files.

Direct and modal transient response analysis methods are implemented as follows.

## Linear Direct Transient Response

The equation of motion is solved directly using the Newmark Beta method.

The use of complex coefficients for damping is not allowed in transient response analysis. Therefore, structural damping is included using equivalent viscous damping.

- ${C}_{1}$
- Matrix of the viscous damper elements, plus the external damping matrices input through the DMIG Bulk Data Entry.
- $G$
- Overall structural damping (PARAM,
`G`). - ${\omega}_{3}$
- Frequency of interest for the conversion of the overall structural
damping into equivalent viscous damping (PARAM,
`W3`). - ${\omega}_{4}$
- Frequency of interest for the conversion of the element structural
damping into equivalent viscous damping (PARAM,
`W4`). - ${C}_{GE}$
- Contribution from structural element damping coefficients $GE$.

`TMTD`field on the TSTEP Bulk Data Entry.

- Traditional Method (Default –
`TMTD`is blank) - Newmark-Beta Method (
`TMTD`= 1)

`TMTD`field to 1 on the TSTEP Bulk Data Entry for Linear Direct Transient Analysis.

- $M$, $C$, and $K$
- Mass, viscous damping, and stiffness matrix, respectively.
- $f$
- Total force.
- $\beta $ and $\gamma $
- Can be modified via the
`TC2`and`TC3`fields of the TSTEP Bulk Data Entry. - $h$
- Timestep.

### Automatic Time Stepping

The Linear Transient solution provides automatic time stepping based on Local
Truncation Error (LTE) for the Newmark-Beta time integration scheme. This can be
controlled using the `MREF` field of the TSTEP
Bulk Data Entry.

Where, $\Vert {u}_{R}\Vert $ is the maximum value of the displacement norm over all the previous time steps.

Where, ${u}_{j}$ is the displacement at time step $j$.

`TOL`is the user-defined tolerance set on the TSTEP Bulk Data Entry):

- If $$\tilde{e}$$ >
`TOL`: Reject current step, cutback to half the current time step, and redo the current step. - If
`TOL`> $$\tilde{e}$$ > 0.5 *`TOL`: Accept current step, cutback the next time step to half the current time step. - If 0.5 *
`TOL`> $$\tilde{e}$$ > 1/16 *`TOL`: No changes. - If 1/16 *
`TOL`> $$\tilde{e}$$: The next time step is enlarged to 1.25 times the current time step.

The `MREF` continuation line on TSTEP entry can
be used to control automatic time stepping, so that the time step $h$ is adjusted according to the LTE of the current
step. As shown above, when error is "large" when compared to the tolerance
(`TOL`), $h$ will be reduced by half and the current step is
re-calculated. The maximum number of such operations within each step is controlled
by the `TN1` field. On the other hand, when $h$ is "small" compared to the tolerance
(`TOL`), $h$ is requested to be increased, but only after TN2
contiguous steps with such a request, will $h$ be actually increased.

### Run Linear Transient 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 statement and a DLOAD statement in a SUBCASE. Similar to mechanical loads, temperature loads (TEMP/TEMPD/TEMPADD) can be applied to Linear Transient Analysis via TLOAD1/TLOAD2 Bulk Data Entries referenced on a DLOAD Subcase Information Entry.

Inertia relief is not supported for Linear Transient Analysis. OptiStruct will error out if this is attempted.

Only one transient subcase can be defined. Initial conditions need to be referenced through the
IC Subcase statement. The analysis time step and termination
time need to be defined through a TSTEP(TIME)
subcase reference. The corresponding time integration scheme can be selected via the
`TMTD` field on the TSTEP entry. Automated
time-stepping is controlled via the `MREF` field on
TSTEP entry. `MREF` = 0
turns off automatic time-stepping and `MREF`=1
activates automated time-stepping.

In addition to the various damping elements and material damping, uniform structural damping $G$ can be applied using PARAM,
`G`.

## Linear Modal Transient Response

In the modal method, a normal modes analysis to obtain the eigenvalues ${\lambda}_{i}={\omega}_{i}^{2}$ and the corresponding eigenvectors $A={A}_{i}$ of the system is performed first.

The modal mass matrix ${A}^{T}MA$ and the modal stiffness matrix ${A}^{T}KA$ are diagonal. This way the system equation is reduced to a set of uncoupled equations for the components of $v$ that can be solved easily.

Here, the matrices ${A}^{T}CA$ are generally non-diagonal. Then coupled problem is similar to the system solved in the direct method, but of a much lesser degree of freedom. The solution of the reduced equation of motion is performed using the Newmark method.

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

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

### 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 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.
- The applied load method generates a maximum of two residual vectors which are the dynamic load vector at 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.

### Run Linear Modal Transient Analysis

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 Entry section using an SPC statement and a DLOAD statement in a SUBCASE. Similar to mechanical loads, temperature loads (TEMP/TEMPD/TEMPADD) can be applied to Linear Transient Analysis via TLOAD1/TLOAD2 Bulk Data Entries referenced on a DLOAD Subcase Information Entry.

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. Residual vectors are also calculated for viscous damping DOF. These are created by default and can be turned off with the RESVEC option NODAMP. 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 can be applied to
unconstrained models. A SUPORT1 Subcase Information 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.

Only one transient subcase can be defined. Initial conditions cannot be defined if the modal method is used. 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 data.

The analysis time step and termination time need to be defined through a TSTEP(TIME) subcase reference. 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 $$G$$ is applied using PARAM,
`G`.

Modal damping can be applied using the SDAMPING reference of a damping table TABDMP1.

## Output

The results of a transient response analysis are displacements, velocities, accelerations, forces, stresses, and strains.

The responses are usually time-dependent. The usual output entries like STRESS, STRAIN, DISPLACEMENT, etc. can be used to request corresponding output values. The NLLOAD I/O Options Entry can be used to request the output of nonlinear loads for each time step.

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.

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).

## Linear Transient Analysis by Fourier Transformation

With the Fourier transformation method, Frequency Response Analysis can be used for the Transient Analysis. The Fourier transformation method may be used to solve the transient response of structural models under periodic loads.

A typical application for this method is a vehicle on a bumpy road.

Time-dependent applied loads are transformed into the frequency domain and all frequency dependent matrix calculations are completed. The frequency response results are then transformed back into the time domain.

The matrix $K$ is the stiffness matrix, the matrix $M$ is the mass matrix, and the matrix $C$ is the damping matrix formed by the damping elements. Initial conditions cannot be defined.

Where, $h(\Omega )$ is the frequency response due to unit load.

- The system has to be reasonably well damped. Too little damping may lead to incorrect results.
- The forcing function should be zero for some time interval to allow decay.
- The frequency interval should follow:
(27) $\text{\Delta}\Omega \le \frac{1}{{T}_{pulse}+{T}_{decay}}$

The direct and modal methods are implemented. The Linear Transient Analysis using Fourier Transformation cannot be used in a model, which also contains a Modal Frequency Response Analysis subcase. OptiStruct will error out in such cases.

### Input/Output

#### Direct Method

Direct frequency response analysis is applied (Frequency Response Analysis).

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 Entry section using an SPC and DLOAD statement in a SUBCASE.

Inertia relief is not implemented for direct frequency response. The solver will error out if it is attempted.

A frequency set must be referenced using a FREQUENCY statement. Initial conditions cannot be applied. The analysis time step and termination time need to be defined through a TSTEP(FOURIER) subcase reference.

In addition to the various damping elements and material damping, uniform structural
damping $$G$$ can be applied using PARAM,
`G`.

#### Modal Method

Modal Frequency Response Analysis is applied (Frequency Response Analysis).

Transient response 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 Entry 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 Information
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. Initial conditions cannot be defined. A METHOD statement is required for the modal method to control the normal modes analysis. The analysis time step and termination time need to be defined through a TSTEP(FOURIER) Subcase reference. 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 can be applied using the SDAMPING reference of a
damping table TABDMP1. The parameter PARAM,
`KDAMP` is to define the method of applying the damping
table.

#### Output

The results for Linear Transient Analysis via Fourier transformation are displacements, velocities, and accelerations. Time-based results are output by default (TIME option) and, for supported output entries, frequency-based results can be requested using the FREQ option in the corresponding I/O Options Entry (for example, DISPLACEMENT(FREQ)).