Configuring a random response procedure

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

2. On the Basic and Damping tabbed pages, configure settings such as frequency range and damping definitions as described in the following procedures.

3. The power spectral density of the Mises equivalent stress and the root mean square of the Mises equivalent stress are computed in the Visualization module. To obtain these data, you must request specific field and history output.

   1. Display the output request editors as described in Creating an output request.
   2. For the field output request of the previous frequency step, select the stress component and invariants (S) output variable.
   3. For the history output request of the random response step, do the following:

      • Select Set as the Domain, and select the desired set from the list.

      • To obtain the power spectral density of the Mises equivalent stress, select the MISES output variable.

      • To obtain the root mean square of the Mises equivalent stress, select the RMISES output variable.

   4. You can view the MISES and RMISES output variables in the Visualization module.

      • To obtain contour plots of the MISES and RMISES output variables, see Selecting the primary field output variable.

      • X–Y data plots can be obtained for the MISES and RMISES output variables at element nodal and unique nodal output variable positions. To obtain these plots, see Reading X–Y data from output database field output.

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. Choose a Scale option to indicate whether you want the frequency range(s) of interest to be divided using a Logarithmic or Linear scale.

4. Enter the following data in the 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 between eigenfrequencies at which the response should be calculated, 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 the value given is less than two (or omitted), the default value of 20 points is assumed. Accurate RMS values can be obtained only if enough points are used so that Abaqus/Standard can integrate accurately over the frequency range.

   Bias

   The bias parameter. This parameter is useful only if you request results at 4 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, since the ends of each interval are the eigenfrequencies where the response amplitudes vary most rapidly. The default bias parameter is 3.0. For more information, see The bias parameter.

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

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 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, $\xi$, 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, $\xi$.

   • 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, ${\alpha }_M$.

        • Beta: stiffness proportional damping, ${\beta }_M$.

   • 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.

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

4. If you selected Frequencies 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, $\xi$, 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, $\xi$.

   • 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, ${\alpha }_M$.

        • Beta: stiffness proportional damping, ${\beta }_M$.

   • 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.

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

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

When you have finished configuring settings for the step, click OK to close the Edit Step dialog box.

You can view the root mean square of the Mises equivalent stress in the Visualization module, view the RMISES output variable from the Field Output dialog box, or create X–Y data from ODB field output. For more information on viewing field output, see Selecting the field output to display, and Reading X–Y data from output database field output.