A transient model dynamic analysis gives the response of the model as a
function of time based on a given time-dependent loading. The structure's
response is based on a subset of the modes of the system, which must first be
extracted using an eigenfrequency extraction procedure (described in
Configuring a frequency procedure).
For more information, see
Transient modal dynamic analysis.
Display the Edit Step dialog box following the
procedure outlined in
Creating a step
(Procedure type:Linear perturbation; Modal
dynamics), or
Editing a step.
On the Basic and Damping
tabbed pages, configure settings such as whether or not to carry over initial
conditions from the results of the preceding step and damping at particular
modes or frequencies as described in the following procedures.
Configure settings on the Basic tabbed page
In the Edit Step dialog box, display the
Basic tabbed page.
In the Description field, enter a short
description of the analysis step.
Abaqus
stores the text that you enter in the output database, and the text is
displayed in the state block by the Visualization module.
Indicate whether or not you want to carry over initial conditions from
the immediately preceding step:
Choose Use initial conditions (when
applicable) if you want
Abaqus/Standard
to carry over initial conditions from the immediately preceding step, which
must be either another modal dynamic step or a static perturbation step:
If the immediately preceding step is a modal dynamic step,
both the displacements and velocities are carried over from the end of that
step and used as initial conditions for the current step.
If the immediately preceding step is a static perturbation
step, the displacements are carried over from that step. If initial velocities
have been defined (Initial conditions in Abaqus/Standard and Abaqus/Explicit),
they will be used; otherwise, the initial velocities will be zero.
Choose Zero initial conditions If you want
the modal dynamic step to begin with zero initial displacements. If you have
defined initial velocities
Abaqus/Standard
will use them; otherwise, the initial velocities will be zero.
In the Time period field, enter the time period
of the step.
In the Time increment field, enter a value for
the desired time increment size.
Configure settings on the Damping tabbed
page
In the Edit Step dialog box, display the
Damping tabbed page.
Choose Specify damping over ranges of Modes
to provide damping values for specific mode ranges.
Choose Specify damping over ranges of
Frequencies to provide damping values at specific frequencies.
Abaqus/Standard
interpolates the damping coefficient for a mode linearly between the specified
frequencies
If you omit damping data on the Damping tabbed
page,
Abaqus/Standard
assumes zero damping values. For more information, see
Specifying modal damping.
If you selected Modes in Step 2, select one or
more of the following options for defining damping:
Display the Direct modal tabbed page to
specify the fraction of critical damping, ,
for a particular mode range, and do the following:
Toggle on Use direct damping data.
Enter the following in the data table:
Start Mode: the mode number of the
lowest mode of a range.
End Mode: the mode number of the
highest mode of a range.
Critical Damping Fraction: fraction
of critical damping, .
Display the Composite modal tabbed page to
select composite modal damping using the damping coefficients calculated in the
preceding frequency step. (The damping calculations performed in the frequency
step are performed using damping data provided in the material definition). Do
the following:
Toggle on Use composite damping data.
Enter the following in the data table:
Start Mode: the mode number of the
lowest mode of a range.
End Mode: the mode number of the
highest mode of a range.
Display the Rayleigh tabbed page to define
Rayleigh damping, and do the following:
Toggle on Use Rayleigh damping data.
Enter the following in the data table:
Start Mode: the mode number of the
lowest mode of a range.
End Mode: the mode number of the
highest mode of a range.