The Theory of Random Vibration in ANSYS

CAE Theoretical
1

Steps for Random Vibration (PSD) Analysis

PSD analysis involves the following six steps:

  1. Build the model;
  2. Obtain modal solution;
  3. Extend modes;
  4. Obtain spectral solution;
  5. Merge modes;
  6. Observe results.

In these six steps, the first two are similar to single-point response spectrum analysis, while the last four steps will be explained in detail below. Random vibration analysis cannot be carried out in the ANSYS/Professional product.

When using the GUI interaction method for the analysis, the Modal Analysis dialog [MODOPT command] includes an option to extend modes [MXPAND command]. Setting this to “YES” allows the following: mode extension. This combines steps 2 (obtaining modal solution) and 3 (extending modes) into one step for computation.

1. Build the Model

This step is similar to other types of analysis, which involves defining work name, analysis title, element type, element real constants, material properties, and model geometry. Note the following two points:

  • Only linear behavior is valid in spectrum analysis. Any nonlinear elements are treated as linear. If contact elements are present, their stiffness is always the initial stiffness and does not change.
  • The material’s elastic modulus [EX] (or other forms of stiffness) and density [DENS] must be defined. Any material nonlinearity will be ignored, but linear, isotropic, or anisotropic material properties are allowed, whether they vary with temperature or not.

2. Obtain Modal Solution

The modal solution (natural frequencies and mode shapes) of the structure is necessary to compute the spectral solution. The specific process for modal analysis is explained in the “Modal Analysis” section. However, note the following:

  • Use the Block Lanczos method (default), Subspace method, or Reduction method to extract modes. Asymmetric, damping, QR damping, and Power Dynamics methods are invalid for the next step of spectral analysis.
  • The number of extracted modes should be sufficient to represent the structure’s response in the frequency range of interest.
  • If using the GUI interactive method, setting the extension mode option to “NO” in the MODOPT dialog will prevent mode extension during modal calculation. Mode extension can be done optionally (refer to the SIGNIF input of the MXPAND command).
  • Material damping must be specified during modal analysis.
  • Freedom constraints must be applied where excitation spectra are applied.
  • After solving, exit the SOLUTION processor.

3. Extend Modes

Whether using the Subspace, Block Lanczos, or Reduction method, mode extension must be performed. More details on mode extension are available in the “Modal Analysis” section of the “Dynamics Analysis Guide.” Additional points to consider:

  • Only extended modes can undergo modal merging in subsequent steps.
  • If interested in stress results from the spectrum, stress calculations must be performed. By default, the mode extension process does not include stress calculations, which means spectral analysis will not output stress data.
  • Mode extension can be performed as a separate solving process or integrated within the modal analysis phase.
  • After mode extension, execute the FINISH command to exit the solver (SOLUTION).

As explained in the “Modal Analysis” section, the MXPAND command can merge modal solving and mode extension into one step (both in GUI interaction and batch methods).

4. Obtain Spectral Solution

When solving the power spectral density (PSD), the system database must contain modal analysis results. The following files must be generated: Jobname.MODE, Jobname.ESAV, Jobname.EMAT, Jobname.FULL (only for Subspace and Block Lanczos methods), and Jobname.RST.

  1. Enter the solver:

    /SOLU
GUI: Main Menu > Solution

  2. For spectrum analysis type (SPOPT command), select Power Spectral Density (PSD).
    If stress results are needed, turn on the stress calculation switch (SPOPT command set to ON). Stress is calculated only if it was requested during mode extension.

  3. Define load step options. The following options apply to random vibration:

    • Spectral data:
      Power Spectral Density (PSD) type
      PSDUNIT
GUI: Main Menu > Solution > Spectrum > -PSD-Settings
      PSD types can include displacement, velocity, force, pressure, or acceleration.
    • Define PSD-Frequency 2D Table
      PSDFREQ, PSDVAL
GUI: Main Menu > Solution > Spectrum > -PSD-PSD vs Freq
      PSDFREQ and PSDVAL commands are used to define the PSD-frequency 2D table.

    Damping types can include Alpha (mass) damping, Beta (stiffness) damping, constant damping ratio, and frequency-dependent damping ratio.

  4. Apply PSD excitation at nodes. A value of 1.0 applies the excitation; 0.0 (or empty) removes the excitation.

    D, DK, DL or DA [Base Excitation]
F or FK [Node Excitation]
LVSCALE [Pressure PSD]
GUI: Main Menu > Solution > -Loads-Apply > -Base PSD Excit-On Nodes

  5. The PFACT command is used to specify the selected PSD table.

5. Merge Modes

During the solution process, modal merging can be performed as a separate step. The basic process is as follows:

/SOLU
GUI: Main Menu > Solution
ANTYPE
GUI: Main Menu > Solution > New Analysis

In random vibration, only the PSD modal merging method is used. This method computes the 1st order displacement, stress, etc. Without executing the PSD command, the program will not calculate the 1st order response of the structure.

6. Observe Results

Random vibration analysis results are written to the results file Jobname.RST, which contains:

  1. Extended mode shapes from the modal analysis;
  2. Static solution for base excitation (PFACT, BASE commands);
  3. If modal merging is requested (PSD command), and if set using the PSDRES command, the following outputs:
    • 1st order displacement solution (displacement, stress, strain, force);
    • 1st order velocity solution (velocity, stress velocity, strain velocity, force velocity);
    • 1st order acceleration solution (acceleration, stress acceleration, strain acceleration, force acceleration).

Results can be viewed in the POST1 processor and, for PSD responses, in POST26.

In POST1, use the SET command to load the desired results, then display them. For example, to load the 1st order displacement solution:

SET
GUI: Main Menu > General Postproc > -Read Results-First Set

In POST26, PSD results can be computed and displayed as follows:

  1. Enter Time-History Postprocessor:
    /POST26
GUI: Main Menu > TimeHist PostPro
  2. Define the response PSD calculations using commands like RPSD, and display the results using PLVAR.

These steps outline the general process of performing a PSD-based random vibration analysis in ANSYS, from model creation to result interpretation.

1 个赞