Configuring a modal dynamics procedure

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.

This task shows you how to:

Create or edit a modal dynamics procedure

  1. Display the Edit Step dialog box following the procedure outlined in Creating a step (Procedure type:Linear perturbation; Modal dynamics), or Editing a step.

  2. 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

  1. In the Edit Step dialog box, display the Basic tabbed page.

  2. 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.

  3. 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.

  4. In the Time period field, enter the time period of the step.

  5. In the Time increment field, enter a value for the desired time increment size.

Configure settings on the Damping tabbed page

  1. In the Edit Step dialog box, display the Damping tabbed page.

    (For information on displaying the Edit Step dialog box, see Creating a step, or Editing a step.)

  2. 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/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.

  3. 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, ξ, for a particular mode range, and 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, ξ.

    • 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:

      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, αM.

        • Beta: stiffness proportional damping, βM.

    For detailed information on how to enter data, see Entering tabular data.

  4. If you selected Frequencies in Step 2, select one or both of the following options for defining damping:

    • Display the Direct modal tabbed page to specify the fraction of critical damping, ξ, 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, ξ.

    • 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, αM.

        • Beta: stiffness proportional damping, βM.

    For detailed information on how to enter data, see Entering tabular data.

  5. If desired, repeat Steps 2–4 to create multiple damping definitions.