Using the AMS eigensolver for a frequency extraction procedure

The Edit Step dialog box provides Basic and Other tabbed pages on which you can specify settings for the AMS eigensolver.

This task shows you how to:

Context:

You can display the Edit Step dialog box following the procedure outlined in Creating a step (Procedure type: Linear perturbation; Frequency), or Editing a step.

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. From the list of Eigensolver options, choose AMS.
  4. Coupling of structural and acoustic regions does not affect a frequency extraction procedure that uses the AMS eigensolver: the structural and acoustic modes are computed as if uncoupled. By default, Abaqus projects structural-acoustic coupling operators defined in the model for use in a later, steady-state dynamic step. To deactivate the projection, toggle off Project acoustic-structural coupling where applicable. Deactivating the coupling operators may improve the analysis speed, but structural-acoustic coupling will then be ignored in subsequent steady-state dynamic steps.
  5. For models that include both structural and acoustic elements, Abaqus by default uses the same frequency range when calculating the acoustic eigenvalues as it does when calculating the structural eigenvalues. To specify different frequency ranges for the two regions, enter an Acoustic range factor. Abaqus multiplies this factor by the Maximum frequency of interest to determine a different maximum frequency for the acoustic region. The minimum frequency remains the same for both regions.
  6. Toggle on Minimum frequency of interest (cycles/time) to specify a lower limit to the frequency range within which Abaqus/Standard will calculate eigenvalues. If you toggle on this option, enter a value for the minimum frequency in the field provided.
  7. In the Maximum frequency of interest (cycles/time) field, enter the upper limit to the frequency range within which Abaqus/Standard will extract all the modes.
  8. Toggle on Limit region of saved eigenvectors if you want to limit eigenvector computation to only the nodes in a particular region. If you toggle on this option, click the arrow to the right of the field provided to select the region of interest.
  9. By default, Abaqus projects any structural or viscous damping operators defined in the model for use in a later, steady-state dynamic step. To deactivate the projection of these operators, toggle off Project damping operators. Deactivating the damping operators may improve the performance of the frequency extraction step; however, structural and viscous material damping will then be ignored in subsequent steady-state dynamic steps. For more information, see Damping in a Mode-Based Steady-State and Transient Linear Dynamic Analysis Using the SIM Architecture.
  10. Toggle on Include residual modes to request that Abaqus/Standard compute residual modes based on the static response of the model to a nominal (or unit) load.

    If you toggle on this option, specify the residual mode regions and the degrees of freedom (DOF) for which you want residual modes calculated. Abaqus/Standard computes one residual mode for every requested degree of freedom.

    For more information, see Residual Modes.

Configure settings on the Other tabbed page

  1. In the Edit Step dialog box, display the Other tabbed page.
  2. Accept the default Matrix storage setting. Since Abaqus/Standard provides eigenvalue extraction only for symmetric matrices, steps with eigenfrequency extraction or eigenvalue buckling prediction procedures always use the symmetric matrix storage and solution scheme. You cannot change this setting. In such steps Abaqus/Standard will symmetrize all contributions to the stiffness matrix.
  3. In the Cutoff multiplier for substructure eigenproblems field, enter A⁢M⁢Scutoff1, the cutoff frequency for substructure eigenproblems, defined as a multiplier of the maximum frequency of interest. The default value is 5.
  4. In the First cutoff multiplier for reduced eigenproblems field, enter A⁢M⁢Scutoff2, the first cutoff frequency for a reduced eigenproblem, defined as a multiplier of the maximum frequency of interest. The default value is 1.6. A⁢M⁢Scutoff2≤A⁢M⁢Scutoff1.
  5. In the Second cutoff multiplier for reduced eigenproblems field, enter A⁢M⁢Scutoff3, the second cutoff frequency for a reduced eigenproblem, defined as a multiplier of the maximum frequency of interest. The default value is 1.3. 1.0≤A⁢M⁢Scutoff3≤A⁢M⁢Scutoff2.

    For more information, see Automatic Multilevel Substructuring (AMS) Eigensolver.

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