Before reading this section, consider becoming familiar with the concepts presented in Structural Static Analysis if you have not already done so.
We will first describe how to do a transient dynamic analysis using the full method. We will then show the steps that differ for the mode-superposition method.
The procedure for a full transient dynamic analysis consists of these steps:
See Building the Model in the Basic Analysis Guide and the Modeling and Meshing Guide.
When building a model for a full transient dynamic analysis:
You can use both linear and nonlinear elements.
Both Young's modulus (EX) (or stiffness in some form) and density (DENS) (or mass in some form) must be defined. Material properties may be linear or nonlinear, isotropic or orthotropic, and constant or temperature-dependent.
You can define damping using element damping, material damping and/or proportional damping ratios. For more information, see Damping.
Some comments about mesh density:
The mesh should be fine enough to resolve the highest mode shape of interest.
Regions where stresses or strains are of interest require a relatively finer mesh than regions where only displacements are of interest.
If you want to include nonlinearities, the mesh should be able to capture the effects of the nonlinearities. For example, plasticity requires a reasonable integration point density (and therefore a fine element mesh) in areas with high plastic deformation gradients.
If you are interested in wave propagation effects (for example, a bar dropped exactly on its end), the mesh should be fine enough to resolve the wave. A general guideline is to have at least 20 elements per wavelength along the direction of the wave.
Before you can perform a full transient dynamic analysis on a model, you need to understand how to establish initial conditions and use load steps.
A transient analysis, by definition, involves loads that are functions of time. To specify such loads, you need to divide the load-versus-time curve into suitable load steps. Each "corner" on the load-time curve may be one load step, as shown in Figure 5.1: Examples of Load-Versus-Time Curves.
The first load step you apply is usually to establish initial conditions. You then specify the loads and load step options for the second and subsequent transient load steps. For each load step, you need to specify both load values and time values, along with other load step options such as whether to step or ramp the loads, use automatic time stepping, and so on. You then write each load step to a file and solve all load steps together. Establishing initial conditions is described below; the remaining tasks are described later in this chapter.
The first step in applying transient loads is to establish initial conditions
(that is, the condition at Time = 0). A transient dynamic analysis requires either
two sets of initial conditions (because the equations being solved are of second
order): initial displacement (
), initial velocity (
), and initial acceleration (
). If no special action is taken, 
, 
, and 
are assumed to be zero.
Note: The term initial displacement as it appears in the following text can be any combination of displacement and force loads. Also, all load steps in the example input fragments that are run without applied transient effects (TIMINT,OFF) should be converged.
Zero initial conditions -- These are the
default conditions; that is, if 
, you do not need to specify anything. You may apply the loads
corresponding to the first corner of the load-versus-time curve in the first load
step.
Nonzero initial conditions -- You can set displacement, velocity, and acceleration initial conditions with the IC and ICROTATE commands.
Caution: Be careful not to define inconsistent initial conditions. For example, if you define an initial velocity at a single degree of freedom, the initial velocity at every other degree of freedom will be 0.0, potentially leading to conflicting initial conditions. In most cases, you will want to define initial conditions at every unconstrained degree of freedom in your model. If these conditions are not the same at every degree of freedom, it is usually much easier to define initial conditions explicitly, as documented below (rather than by using the IC command).
See the Command Reference for a discussion of the TIMINT and IC commands.
Nonzero initial displacement and
nonzero initial velocity - Because the IC command
only supports one condition at a given degree of freedom (displacement, velocity, or
acceleration), the nonzero velocity is established by applying displacements over a
time interval on the part of the structure where velocity is to be specified. For
example, if = 1.0 and 
= 2.5, you would apply a displacement of 1.0 over a time interval
of 0.4:
... TIMINT,OFF ! Time integration effects off D,ALL,UY,1.0 ! Initial displacement = 1.0 TIME,.4 ! Initial velocity = 1.0/0.4 = 2.5 SOLVE DDELE,ALL,UY ! Remove imposed displacements TIMINT,ON ! Time integration effects on ...
You can use the ICROTATE command to specify initial velocity at nodes as a sum of rotation about an axis and translation. The command calculates the nodal velocities and saves them in the database as if the IC command had been used to calculate these velocities. Thus, when the Jobname.cdb or Jobname.db file is written, the velocities prescribed by the ICROTATE command appear as IC commands. The last defined IC or ICROTATE command overwrites the initial conditions specified by the preceding command.
This step for a transient dynamic analysis is the same as for a basic structural analysis (see Set Solution Controls in Structural Static Analysis) with the following additions:
If you need to establish initial conditions for the full transient dynamic analysis (as described in Establish Initial Conditions), you must do so for the first load step of the analysis. You can then cycle through the Solution Controls dialog box additional times to set individual load step options for the second and subsequent load steps (as described in Repeat Steps 3-6 for Each Load Step).
To access the Solution Controls dialog box, select menu path . The following sections provide brief descriptions of the options that appear on each tab of the dialog box. For details about how to set these options, select the tab that you are interested in and then click the button. Nonlinear Structural Analysis also contains details about the nonlinear options introduced in this chapter.
The Basic tab is active when you access the dialog box.
The controls that appear on the Basic tab provide the minimum amount of data needed for the analysis. Once you are satisfied with the settings on the Basic tab, you do not need to progress through the remaining tabs unless you want to adjust the default settings for the more advanced controls. As soon as you click on any tab of the dialog box, the settings are applied to the database and the dialog box closes.
You can use the Basic tab to set the options listed in Table 2.1: Basic Tab Options. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Basic tab, and click the button.
Special considerations for setting these options in a full transient analysis include:
When setting ANTYPE and NLGEOM, select Small Displacement Transient if you are performing a new analysis and you want to ignore large deformation effects such as large deflection, large rotation, and large strain. Select Large Displacement Transient if you expect large deflections (as in the case of a long, slender bar under bending) or large strains (as in a metal-forming problem). Select Restart Current Analysis if you want to restart a failed nonlinear analysis, or if you have previously completed a static prestress or a full transient dynamic analysis and you want to extend the time-history.
When setting AUTOTS, remember that this load step option (which is also known as time-step optimization in a transient analysis) increases or decreases the integration time step based on the response of the structure. For most problems, we recommend that you turn on automatic time stepping, with upper and lower limits for the integration time step. These limits, specified using DELTIM or NSUBST, help to limit the range of variation of the time step; see Automatic Time Stepping for more information. The default is ON.
NSUBST and DELTIM are load step options that specify the integration time step for a transient analysis. The integration time step is the time increment used in the time integration of the equations of motion. You can specify the time increment directly or indirectly (that is, in terms of the number of substeps). The time step size determines the accuracy of the solution: the smaller its value, the higher the accuracy. You should consider several factors in order to calculate a "good" integration time step; see Guidelines for Integration Time Step for details.
When setting OUTRES, keep this caution in mind:
Caution: By default, only the last substep (time-point) is written to the results file (Jobname.rst) in a full transient dynamic analysis. To write all substeps, set the Frequency so that it writes all of the substeps.
You can use the Transient tab to set the options listed in Table 5.1: Transient Tab Options. For specific information about using the Solution Controls dialog box to set these options, access the dialog box, select the Transient tab, and click the button.
Table 5.1: Transient Tab Options
| Option | For more information about this option, see: |
|---|---|
| Specify whether time-integration effects are on or off (TIMINT) | |
| Specify whether to ramp the load change over the load step or to step-apply the load change (KBC) | |
| Specify mass and stiffness damping (ALPHAD, BETAD) |
|
| Specify midstep criterion (MIDTOL) | |
| Select the time-integration method, Newmark or HHT (TRNOPT) | |
| Define integration parameters (TINTP) |
Special considerations for setting these options in a full transient analysis include:
TIMINT is a dynamic load step option that specifies whether time-integration effects are on or off. Time integration effects must be turned on for inertia and damping effects to be included in the analysis (otherwise a static solution is performed), so the default is to include time-integration effects. This option is useful when beginning a transient analysis from an initial static solution; that is, the first load steps are solved with the time-integration effects off.
ALPHAD (alpha, or mass, damping) and BETAD (beta, or stiffness, damping) specify damping options. Damping in some form is present in most structures and should be included in your analysis. See Damping Option for other damping options.
TRNOPT (
TINTOPT) specifies the time-integration method to be used. The default is Newmark method.TINTP specifies transient integration parameters. These parameters control the nature of the Newmark and HHT time-integration techniques. Alternatively, you can specify the intended application for the analysis using this command, and the program will automatically set the appropriate transient analysis settings.
The options on the remaining tabs in the Solution Controls dialog box for a full transient analysis are the same as the ones you can set for a static structural analysis. See the following sections of Structural Static Analysis for a list of these options:
Using the Advanced NL Tab. Exception: You cannot use arc-length options in a full transient analysis.
The additional solution options that you can set for a full transient analysis are mostly the same as the ones you can set for a static structural analysis. For a general description of what additional solution options are, along with descriptions of those options that are the same, see the following sections of Structural Static Analysis:
Additional solution options for a full transient analysis that differ from those for a static analysis, or have different descriptions are presented in the following sections.
You may also use the NLHIST command to monitor results of interest in real time during solution. Before starting the solution, you can request nodal data such as displacements or reaction forces at specific nodes. You can also request element nodal data such as stresses and strains at specific elements to be graphed. Pair-based contact data are also available. The result data are written to a file named Jobname.nlh.
For example, a reaction force-deflection curve could indicate when possible buckling behavior occurs. Nodal results and contact results are monitored at every converged substep while element nodal data are written as specified via the OUTRES setting.
You can also track results during batch runs. To
execute, either access the Launcher and select Run Results Tracker
Utility from the Tools menu, or type
nlhist242 at the command
line. Use the supplied file browser to navigate to your
Jobname.nlh file, and click on it to invoke the
tracking utilty. You can use this utilty to read the file at any time, even
after the solution is complete.
To use this option, use either of these methods:
You may include prestress effects in your analysis. This requires element files from a previous static (or transient) analysis; see Performing a Prestressed Transient Dynamic Analysis for details.
Use this load step option to include damping. Damping in some form is present in most structures and should be included in your analysis. In addition to setting ALPHAD and BETAD on the Solution Controls dialog box (as described in Using the Transient Tab), you can specify the following additional forms of damping for a full transient dynamic analysis:
To use the MP form of damping:
Use this analysis option to specify a lumped mass matrix formulation. We recommend the default formulation for most applications. However, for some problems involving "skinny" structures, such as slender beams or very thin shells, the lumped mass approximation might provide better results. Also, the lumped mass approximation can result in a shorter run time and lower memory requirements.
To use this option:
You are now ready to apply loads for the analysis. The loads shown in Table 2.5: Loads Applicable in a Static Analysis are also applicable to a transient dynamic analysis. In addition to these, you can apply acceleration loads in a transient analysis (see Degree-of-Freedom Constraints in the Basic Analysis Guide for more information).
Except for inertia loads, velocity loads, and acceleration loads, you can define loads either on the solid model (keypoints, lines, and areas) or on the finite element model (nodes and elements). In an analysis, loads can be applied, removed, operated on, or deleted. For a general discussion of solid-model loads versus finite-element loads, see Loading in the Basic Analysis Guide.
You can also apply time-dependent boundary conditions by defining a one-dimensional table (TABLE type array parameter). See Applying Loads via Tabular Input.
Note: It is recommended that you use acceleration input to define support motion
when applicable (using the tabular array parameter definition on
the D,,ACC
or ACEL command). A displacement input
(D,,U command) is likely to show numerical noise, because
it implies a discontinuity in acceleration in the simulation. In this case,
numerical damping (GAMMA on
the TINTP command) can be used to improve the
acceleration and force results.
As described in Establish Initial Conditions, you need to apply loads and save the load configuration to a load step file for each corner of the load-versus-time curve. You may also want to have an additional load step that extends past the last time point on the curve to capture the response of the structure after the transient loading.
For each load step that you want to define for a full transient dynamic analysis, you need to repeat steps 3-6. That is, for each load step, reset any desired solution controls and options, apply loads, and write the load configuration to a file.
For each load step, you can reset any of these load step options: TIMINT, TINTP, ALPHAD, BETAD, MP,ALPD, MP,BETD, TIME, KBC, NSUBST, DELTIM, AUTOTS, NEQIT, CNVTOL, PRED, LNSRCH, CRPLIM, NCNV, CUTCONTROL, OUTPR, OUTRES, ERESX, and RESCONTROL.
An example load step file is shown below:
TIME, ... ! Time at the end of 1st transient load step Loads ... ! Load values at above time KBC, ... ! Stepped or ramped loads LSWRITE ! Write load data to load step file TIME, ... ! Time at the end of 2nd transient load step Loads ... ! Load values at above time KBC, ... ! Stepped or ramped loads LSWRITE ! Write load data to load step file TIME, ... ! Time at the end of 3rd transient load step Loads ... ! Load values at above time KBC, ... ! Stepped or ramped loads LSWRITE ! Write load data to load step file Etc.
Save a copy of the database to a named file. You can then retrieve your model by reentering the program and issuing RESUME.
Use one of these methods to start the transient solution:
For additional ways to create and solve multiple load steps (the array parameter method and the multiple SOLVE method), see Solving Multiple Load Steps in the Basic Analysis Guide.
Use one of these methods to exit the solution processor:
You review results for a full transient analysis in the same way that you view review results for most structural analyses.
Also see Appendix B: Example: Energy Calculations in Transient and Harmonic Analyses.
You can review these results using either POST26, which is the time-history postprocessor, or POST1, which is the general postprocessor.
POST26 is used to review results at specific points in the model as functions of time.
POST1 is used to review results over the entire model at specific time points.
Some typical postprocessing operations for a transient dynamic analysis are explained below. For a complete description of all postprocessing functions, see Postprocessors Available in the Basic Analysis Guide.
The points to remember for a full transient analysis are the same as those for most structural analyses. See Hints and Tips in Structural Static Analysis.
POST26 works with tables of result item versus time, known as variables. Each variable is assigned a reference number, with variable number 1 reserved for time.
Define the variables.
Command(s): NSOL (primary data, that is, nodal displacements) ESOL (derived data, that is, element solution data, such as stresses) RFORCE (reaction force data) FORCE (total force, or static, damping, or inertia component of total force) SOLU (time step size, number of equilibrium iterations, response frequency, and so on)GUI:Graph or list the variables. By reviewing the time-history results at strategic points throughout the model, you can identify the critical time points for further POST1 postprocessing.
Many other postprocessing functions, such as performing math operations among variables, moving variables into array parameters, and moving array parameters into variables, are available in POST26. See The Time-History Postprocessor (POST26) in the Basic Analysis Guide for details.
Read in model data from the database file.
Read in the desired set of results. Use the SET command to identify the data set by load step and substep numbers or by time.
Perform the necessary POST1 operations. The typical POST1 operations that you perform for a transient dynamic analysis are the same as those that you perform for a static analysis. See Typical Postprocessing Operations for a list of these operations.
Note: If you specify a time for which no results are available, the results that are stored will be a linear interpolation between the two nearest time points.
! Build the Model /FILNAM,... ! Jobname /TITLE,... ! Title /PREP7 ! Enter PREP7 --- ---! Generate model --- FINISH ! Apply Loads and Obtain the Solution /SOLU ! Enter SOLUTION ANTYPE,TRANS ! Transient analysis TRNOPT,FULL ! Full method D,... ! Constraints F,... ! Loads SF,... ALPHAD,... ! Mass damping BETAD,... ! Stiffness damping KBC,... ! Ramped or stepped loads TIME,... ! Time at end of load step AUTOTS,ON ! Auto time stepping DELTIM,... ! Time step size OUTRES,... ! Results file data options LSWRITE ! Write first load step --- ---! Loads, time, etc. for 2nd load step --- LSWRITE ! Write 2nd load step SAVE LSSOLVE,1,2 ! Initiate multiple load step solution FINISH ! ! Review the Results /POST26 SOLU,... ! Store solution summary data NSOL,... ! Store nodal result as a variable ESOL,,,, ! Store element result as a variable RFORCE,... ! Store reaction as a variable PLVAR,... ! Plot variables PRVAR,... ! List variables FINISH /POST1 SET,... ! Read desired set of results into database PLDISP,... ! Deformed shape PRRSOL,... ! Reaction loads PLNSOL,... ! Contour plot of nodal results PRERR ! Global percent error (a measure of mesh adequacy) --- ---! Other postprocessing as desired --- FINISH
See the Command Reference for discussions of the ANTYPE, TRNOPT, ALPHAD, BETAD, KBC, TIME, AUTOTS, DELTIM, OUTRES, LSWRITE, LSSOLVE, SOLU, NSOL, ESOL, RFORCE, PLVAR, PRVAR, PLDISP, PRRSOL, PLNSOL, and PRERR commands.