Inserting a New Mode-based Steady-State Dynamics Step

Inserting a mode-based steady-state dynamic analysis step within the Simulation History enables you to calculate the steady-state dynamic linearized response of a system to harmonic excitation. Abaqus calculates the response based on the system's eigenfrequencies and modes, which must first be extracted by using the eigenfrequency extraction procedure in a Frequency step. This type of procedure is less expensive computationally than subspace-based steady-state analysis, but it is less accurate, in particular if significant material damping is present.

Mode-based steady-state dynamic steps are available only in a Nonlinear Structural case. They can be defined in new cases or in cases that contain other general static or static linear perturbation steps. Mode-based steady-state dynamic steps cannot be defined in an Explicit Dynamics case or in a Thermal case. See Step Sequence Restrictions for more information.

This task shows you how to insert a new Mode-based Steady-State Dynamics step in a Nonlinear Structural case.

Select Start>Analysis & Simulation>Nonlinear Structural Analysis from the menu bar to enter the Nonlinear Structural Analysis workbench.
From the New Analysis Case dialog box, select Nonlinear Structural Case.
Click the Steady-State Dynamics Step: Mode icon .
Tip: Alternatively, you can select Insert>Steady-State Dynamics Step: Modal from the menu bar, or you can right-click the last step in the simulation history and select Insert Step Below>Steady-State Dynamics Step: Modal from the menu that appears.
The Steady-State Dynamics Step: Modal dialog box appears, and a Steady State Dynamics Step: Mode objects set appears in the specification tree under the Simulation History objects set for the current Nonlinear Structural case.
You can change the step identifier by editing the Step name field. This name will be used in the specification tree.
Enter a description for the step in the Step description field.
Choose a Frequency scale option to indicate whether you want the frequency range(s) of interest to be divided using a Logarithmic or Linear scale.
From the Interval options, do one of the following:
- Select Eigenfrequency to subdivide the frequency range(s) of interest using the system's eigenfrequencies.
- Select Range to subdivide the frequency range(s) of interest using the number of points you specify in the Frequency sampling data table.
Enter the following data in the Frequency sampling data table:
Lower Frequency
The lower limit of the frequency range or a single frequency, in cycles/time.
Upper Frequency
The upper limit of the frequency range, in cycles/time. If you enter zero, Abaqus/Standard assumes that results are required only at the frequency specified in the Lower Frequency column.
Number of Points
The number of points in the frequency range at which results should be given.
If you selected Eigenfrequency as the sampling Interval, this value is the number of points at which results should be given, including the end points, from the lower limit of the frequency range to the first eigenfrequency in the range; in each interval from eigenfrequency to eigenfrequency; and from the highest eigenfrequency in the range to the high limit of the frequency range.
If you selected Range as the sampling Interval, this value is the total number of points in the frequency range, including the end points.
Bias
The bias parameter. This parameter is useful only if you request results at four or more frequency points. It is used to bias the results points toward the ends of the intervals so that better resolution is obtained there. This option is recommended if you have selected Eigenfrequency as the sampling Interval, since the ends of each interval are the eigenfrequencies where the response amplitudes vary most rapidly.
If you want to provide global damping values, do the following:
1. Toggle on Use global damping data.
2. Enter any of the following values:
  - For the Alpha option, specify a value for the first Rayleigh damping ratio.
  - For the Beta option, specify a value for the second Rayleigh damping ratio.
  - For the Structural option, specify a value for the structural damping ratio.
Indicate how you want to provide damping values:
- 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 interpolates the damping coefficient for a mode linearly between the specified frequencies
If you omit damping data on the Damping tabbed page, Abaqus assumes zero damping values.
If you selected Modes in Step 10, select one or more of the following options for defining damping:
- Toggle on Direct to display the Direct tabbed page, then specify the fraction of critical damping, for a particular mode range. Do the following:
  1. Toggle on Use direct damping data.
  2. 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 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:
  1. Toggle on Use composite damping data.
  2. 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:
  1. Toggle on Use Rayleigh damping data.
  2. 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.
    - Alpha: mass proportional damping, .
    - Beta: stiffness proportional damping, .
- Display the Structural tabbed page to define damping that is proportional to the internal forces but opposite in direction to the velocity. Do the following:
  1. Toggle on Use structural damping data.
  2. 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.
    - Damping constant: Damping factor, s.
If you selected Frequencies in Step 10, select one or more of the following options for defining damping:
- Display the Direct tabbed page to specify the fraction of critical damping, for a particular frequency range. Do the following:
  1. Toggle on Use direct damping data.
  2. Enter the following in the data table:
    - Frequency: frequency value in cycles/time.
    - Critical damping fraction: fraction of critical damping, .
- Display the Rayleigh tabbed page to define Rayleigh damping, and do the following:
  1. Toggle on Use Rayleigh damping data.
  2. Enter the following in the data table:
    - Frequency: frequency value in cycles/time.
    - Alpha: mass proportional damping, .
    - Beta: stiffness proportional damping, .
- Display the Structural tabbed page to define damping that is proportional to the internal forces but opposite in direction to the velocity. Do the following:
  1. Toggle on Use structural damping data.
  2. Enter the following in the data table:
    - Frequency: frequency value in cycles/time.
    - Damping constant: Damping factor, s.
If desired, repeat Steps 11–12 to create multiple damping definitions.
Click OK when you have finished defining the step.
The Steady-State Dynamics Step (Modal) objects set contains a default Field Output Request object in a Field Output Requests objects set. See Requesting Results for more information.