Using the Lanczos eigensolver for a frequency extraction procedure

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 Lanczos.

4. Choose one of the Number of eigenvalues requested options to indicate how many eigenvalues you want calculated:

   • Choose All in frequency range if you want Abaqus/Standard to calculate all the eigenvalues within a range determined by a maximum frequency value (and, if desired, a minimum frequency value) that you enter.

   • Choose Value if you want a particular number of eigenvalues to be calculated. Enter that value in the field provided.

5. Toggle on Frequency shift (cycles/time)**2 to specify a positive or negative shifted squared frequency, S. If you toggle this option on, enter a value for the frequency shift in the field provided. For more information, see Frequency shift.

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.

   This option is required if you intend to use the Lanczos solver in parallel mode.

7. Toggle on Maximum frequency of interest (cycles/time) to specify an upper limit to the frequency range within which Abaqus/Standard will calculate eigenvalues. If you toggle on this option, enter a value for the maximum frequency in the field provided.

   This option is required if you intend to use the Lanczos solver in parallel mode.

8. If the model includes acoustic and structural elements coupled together or ASI-type elements, you can toggle on Include acoustic-structural coupling where applicable to include the effect of acoustic-structural coupling during the frequency extraction. (This option is toggled on by default.) For more information, see Structural-acoustic coupling.

9. Specify your preference for block size:

   • Choose Default to use the default block size of 7, which is usually appropriate.

   • Choose Value to enter a particular block size. Enter the value in the field provided. In general, the block size for the Lanczos method should be as large as the largest expected multiplicity of eigenvalues.

   For more information, see Lanczos eigensolver.

10. Specify your preference for the Maximum number of block Lanczos steps:

    • Choose Default to allow Abaqus/Standard to determine the number of block Lanczos steps within each Lanczos run. The default value is usually appropriate.

    • Choose Value to enter a limit to the number of Lanczos steps within each Lanczos run. Enter the value in the field provided. In general, if a particular type of eigenproblem converges slowly, providing more block Lanczos steps will reduce the analysis cost. On the other hand, if you know that a particular type of problem converges quickly, providing fewer block Lanczos steps will reduce the amount of in-core memory used.

11. Toggle on Use SIM-based linear dynamics procedures to activate the high performance, mode-based linear dynamics analysis capability. If the eigenmodes that are extracted in this step will be used for subsequent mode-based or subspace-based linear dynamic procedures, the SIM-based capability offers improved efficiency for large models with minimal output requests. For more information, see Using the SIM architecture for modal superposition dynamic analyses.

12. If you toggled on Use SIM-based linear dynamics procedures, Abaqus projects structural and viscous damping operators defined in the model for use in a later, steady-state dynamic step. To deactivate the projection of damping 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.

13. Toggle on Include residual modes to request that Abaqus/Standard compute residual modes based on the loads specified in the immediately preceding static, linear perturbation step. For more information, see Obtaining residual modes for use in mode-based procedures.

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. Choose an option for normalizing eigenvectors:

   • Choose Displacement to normalize the eigenvectors so that the largest displacement, rotation, or acoustic pressure entry in each vector is unity.

   • Choose Mass to normalize the eigenvectors with respect to the structure's mass matrix (the eigenvectors are scaled so that the generalized mass for each vector is unity).

   If you toggled on Use SIM-based linear dynamics procedures on the Basic tabbed page, only mass normalization is available. For more information, see Normalization.

4. Toggle on Evaluate dependent properties at frequency to evaluate frequency-dependent properties for viscoelasticity, springs, and dashpots during the eigenvalue extraction. If you toggle this option on, enter the desired evaluation frequency in the field provided. For more information, see Evaluating frequency-dependent material properties.

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