|
»Click here to display Table of Contents«
|
Linear Transient Analysis |
|
|
|
|
|
Linear Transient Analysis |
|
|
|
|
Transient response analysis is used to calculate 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 transient response analysis computes the structural responses solving the following equation of motion with initial conditions in matrix form.
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.
Direct and modal transient response analysis methods are implemented as follows.
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.
The damping matrix C is composed of several contributions as follows:
Where, C1 is the matrix of the viscous damper elements, plus the external damping matrices input through the DMIG bulk data entry; G is the overall structural damping (PARAM, G); 
is the frequency of interest for the conversion of the overall structural damping into equivalent viscous damping (PARAM, W3); 
is the frequency of interest for the conversion of the element structural damping into equivalent viscous damping (PARAM, W4); and CGE is the contribution from structural element damping coefficients GE.
The transient 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 statement and a DLOAD statement in a SUBCASE.
Inertia relief is not supported for direct transient response 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.
In addition to the various damping elements and material damping, uniform structural damping G can be applied using PARAM, G.
In the modal method, a normal modes analysis to obtain the eigenvalues 
and the corresponding eigenvectors 
of the system is performed first. The state vector u can be expressed as a scalar product of the eigenvectors A and the modal responses v.
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. This way the system equation is reduced to a set of uncoupled equations for the components of v that can be solved easily.
The inclusion of damping yields:
Here, the matrices 
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 Beta method.
The decoupling of the equations can be maintained if the damping is applied to each mode separately. This is done through a damping table TABDMP1 that lists damping values gi versus natural frequency fi .
The decoupled equation is:
or
Where, 
is the modal damping ratio, and 
is the modal eigenvalue.
Three types of modal damping values gi ( fi ) can be defined: G – Structural damping, CRIT – Critical damping, and Q – Quality factor. They are related through the following three equations at resonance:
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.
There are two ways this is implemented.
| • | 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.
Transient 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 statement and a 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. 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 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.
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.
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).
Using the Fourier transformation method, frequency response analysis can be used for the transient analysis. The Fourier transformation method may be used to solve for 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 following equation of motion with initial conditions in matrix form is solved:
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. The load vector is transformed from the time domain into the frequency domain using:
The response in given by:
Where, After the frequency response analysis, the time-dependent response can be recovered using:
For the results to be accurate it is important to note that:
The direct and modal methods are implemented. The Transient Response 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. InputDirect MethodDirect frequency response analysis is applied (Frequency Response Analysis). Transient 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. 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 MethodModal frequency response analysis is applied (Frequency Response Analysis). Transient 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. 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. OutputThe results for Transient Response Analysis via Fourier transformation are displacements, velocities, accelerations, forces, stresses, and strains. Time-based results are output by default 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)). |
Saving and Retrieving Normal Modes Analysis
AMLS (Automatic Multi-Level Sub-structuring) Eigensolver
