To create or edit a static, linear perturbation procedure:

1. Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: Linear perturbation; Static, Linear perturbation), or “Editing a step,” Section 14.9.3.

2. On the Basic and Other tabbed pages, describe the step and enter equation solver preferences as described in the following procedures.

To configure a static, linear perturbation 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. Display the Other tabbed page.

4. Choose an Equation Solver Method option:

   • Choose Direct to use the default direct sparse solver.

   • Choose Iterative to use the iterative linear equation solver. The iterative solver is typically most useful for blocky structures with millions of degrees of freedom. For more information, see “Iterative linear equation solver,” Section 6.1.6 of the Abaqus Analysis User's Guide.

5. Choose a Matrix storage option:

   • Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.

   • Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme.

   • Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.

   For more information on matrix storage, see “Matrix storage and solution scheme in Abaqus/Standard” in “Defining an analysis,” Section 6.1.2 of the Abaqus Analysis User's Guide.

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

To create or edit a buckling procedure:

1. Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: Linear perturbation; Buckle), or “Editing a step,” Section 14.9.3.

2. On the Basic tabbed page, configure settings such as eigensolver extraction method and maximum number of iterations as described in the following procedures.

   The Other tabbed page displays the default matrix storage option. You cannot change this setting because Abaqus/Standard provides eigenvalue extraction for only symmetric matrices. In eigenvalue buckling prediction procedures Abaqus/Standard symmetrizes all contributions to the stiffness matrix.

To 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. Choose either the Lanczos eigensolver or the Subspace iteration eigensolver.

   The Lanczos method is generally faster when a large number of eigenmodes is required for a system with many degrees of freedom. However, this method does have some limitations (see the warning at the bottom of the Basic tabbed page). The subspace iteration method may be faster when only a few (less than 20) eigenmodes are needed. For more information, see “Selecting the eigenvalue extraction method” in “Eigenvalue buckling prediction,” Section 6.2.3 of the Abaqus Analysis User's Guide.

4. In the Number of eigenvalues requested field, enter the number of eigenvalues that you want to be estimated. Significant overestimation of the actual number of eigenvalues can create very large files. If you underestimate the actual number of eigenvalues, Abaqus/Standard will issue a corresponding warning message.

5. If you selected the Lanczos eigensolver, do the following:

   1. Toggle on Minimum eigenvalue of interest to enter a lower limit to the range of eigenvalues Abaqus/Standard will extract. If you toggle on this option, enter the value in the field provided.

   2. Toggle on Maximum eigenvalue of interest to enter an upper limit to the range of eigenvalues Abaqus/Standard will extract. If you toggle on this option, enter the value in the field provided.

      If you specify a range of eigenvalues, Abaqus/Standard will extract eigenvalues until either the requested number of eigenvalues has been extracted in the given range or all the eigenvalues in the given range have been extracted.

   3. Choose a Block size option:

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

      • Choose Value to enter a particular block size 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 “Selecting the eigenvalue extraction method” in “Eigenvalue buckling prediction,” Section 6.2.3 of the Abaqus Analysis User's Guide.

   4. 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. 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.

6. If you selected the Subspace eigensolver, do the following:

   1. Toggle on Maximum eigenvalue of interest to enter an upper limit to the range of eigenvalues Abaqus/Standard will extract. If you toggle on this option, enter the value in the field provided.

      Abaqus/Standard will extract eigenvalues until either the requested number of eigenvalues has been extracted or the last eigenvalue extracted exceeds the maximum eigenvalue of interest.

   2. Enter a value for the number of Vectors used per iteration. In general, the convergence is more rapid with more vectors, but the memory requirement is also larger. Thus, if you know that a particular type of eigenproblem converges slowly, providing more vectors by using this option might reduce the analysis cost.

   3. Enter a value for the Maximum number of iterations. The default is 30.

7. Click OK to save the step and to close the Edit Step dialog box.

To create or edit a complex frequency procedure:

1. Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: Linear perturbation; Complex frequency), or “Editing a step,” Section 14.9.3.

2. On the Basic and Other tabbed pages, configure settings such as the number of eigenvalues requested and matrix solver preferences as described in the following procedures.

To 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. Choose an option for specifying the Number of eigenvalues requested:

   • Choose All if you want Abaqus/Standard to report all the eigenmodes available in the projected subspace, formulated on the basis of all eigenmodes computed in the preceding frequency step.

   • Choose Value to enter a specific number of eigenmodes that you want Abaqus/Standard to report.

4. Toggle on Frequency shift (cycles/time) to specify a shift point, S, for the complex eigenvalue extraction procedure (S ≥ 0). Abaqus/Standard reports the complex eigenmodes, , in order of increasing so that the modes with the imaginary part closest to a given shift point are reported first. This feature is useful when a particular frequency range is of concern. The default is no shift.

5. Toggle on Minimum frequency of interest (cycles/time) to specify a lower limit to the frequency range within which Abaqus/Standard reports eigenmodes.

6. Toggle on Maximum frequency of interest (cycles/time) to specify an upper limit to the frequency range within which Abaqus/Standard reports eigenmodes.

7. Toggle on Include friction-induced damping effects to include friction-induced contributions to the damping matrix. For more information, see “Contact conditions with sliding friction” in “Complex eigenvalue extraction,” Section 6.3.6 of the Abaqus Analysis User's Guide.

To configure settings on the Other tabbed page:

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

   (For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

2. Choose a Matrix solver option:

   • Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.

   • Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme.

   • Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.

   For more information on matrix storage, see “Matrix storage and solution scheme in Abaqus/Standard” in “Defining an analysis,” Section 6.1.2 of the Abaqus Analysis User's Guide.

3. Toggle on Evaluate dependent properties at frequency to enter a frequency at which Abaqus/Standard will evaluate frequency-dependent material properties. For more information, see “Evaluating frequency-dependent material properties” in “Complex eigenvalue extraction,” Section 6.3.6 of the Abaqus Analysis User's Guide.

To create or edit a modal dynamics procedure:

1. Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: Linear perturbation; Modal dynamics), or “Editing a step,” Section 14.9.3.

2. On the Basic, Damping, and Other 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.

To 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,” Section 34.2.1 of the Abaqus Analysis User's Guide), 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.

To 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,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

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” in “Transient modal dynamic analysis,” Section 6.3.7 of the Abaqus Analysis User's Guide.

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, , 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, .

   • 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, .

        • Beta: stiffness proportional damping, .

   For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.

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, , 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, .

   • 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, .

        • Beta: stiffness proportional damping, .

   For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.

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

To configure settings on the Other tabbed page:

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

   (For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

2. Choose an option for Default load variation with time:

   • Choose Instantaneous if you want loads to be applied instantaneously at the start of the step and remain constant throughout the step.

   • Choose Ramp linearly over step if the load magnitude is to vary linearly over the step, from the value at the end of the previous step to the full magnitude of the load.

To create or edit a random response procedure:

1. Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: Linear perturbation; Random response), or “Editing a step,” Section 14.9.3.

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,” Section 14.12.1.

   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,” Section 42.5.3.

      • 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,” Section 47.2.2.

To 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. 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” in “Random response analysis,” Section 6.3.11 of the Abaqus Analysis User's Guide.

   For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.

To 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,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

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” in “Random response analysis,” Section 6.3.11 of the Abaqus Analysis User's Guide.

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, , 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, .

   • 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, .

        • Beta: stiffness proportional damping, .

   • 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,” Section 3.2.7.

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, , 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, .

   • 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, .

        • Beta: stiffness proportional damping, .

   • 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,” Section 3.2.7.

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

To create or edit a response spectrum procedure:

1. Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: Linear perturbation; Response spectrum), or “Editing a step,” Section 14.9.3.

2. On the Basic and Damping tabbed pages, configure settings such as a damping coefficient and the methods for combining multidirectional excitations as described in the following procedures.

To 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. Click the arrow to the right of the Excitations field, and select a directional summation method.

   • For the following options, Abaqus/Standard sums the directional excitation components first and then performs the modal summation:

     • Select Single direction to sum the directional excitation components for a single direction algebraically.

     • Select Multiple direction absolute sum to sum the directional excitation components for multiple directions algebraically.

   • For the following options, Abaqus/Standard performs the modal summation first and then sums the directional excitation components:

     • Select Multiple direction square root of the sum of squares to sum the directional excitation components for multiple directions using the square root of the sum of the squares.

     • Select Multiple direction thirty percent rule to sum the directional excitation components for multiple directions using the 30% rule.

     • Select Multiple direction forty percent rule to sum the directional excitation components for multiple directions using the 40% rule.

   See “Directional summation methods” in “Response spectrum analysis,” Section 6.3.10 of the Abaqus Analysis User's Guide, for more information.

4. Click the arrow to the right of the Summations field, and select a modal summation method. For information on each of the methods, see “Modal summation methods” in “Response spectrum analysis,” Section 6.3.10 of the Abaqus Analysis User's Guide.

5. On the First direction tabbed page (and on the Second direction and Third direction tabbed pages if applicable), do the following:

   1. In the Use response spectrum field, select the spectrum amplitude to use for calculating the response. Alternatively, you can click to create a new amplitude. (See “Defining a spectrum,” Section 57.11,” for more information.)

   2. Enter Direction cosines X, Y, and Z.

   3. In the Scale factor field, enter the factor multiplying the magnitudes in the response spectrum.

   4. In the Time duration field, enter the time duration of the dynamic event from which the spectrum was created. This setting is applicable only when the Double sum combination modal summation method is specified.

   For multiple direction excitations, you have the option of toggling on Apply third direction on the Third direction tabbed page to include data for a third direction.

To 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,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

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” in “Response spectrum analysis,” Section 6.3.10 of the Abaqus Analysis User's Guide.

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, , for a particular mode range. 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, .

   • 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, .

        • Beta: stiffness proportional damping, .

   For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.

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, , 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, .

   • 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, .

        • Beta: stiffness proportional damping, .

   For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.

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

To create or edit a direct-solution steady-state dynamic procedure:

1. Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: Linear perturbation; Steady-state dynamics, Direct), or “Editing a step,” Section 14.9.3.

2. On the Basic and Other tabbed pages, configure settings such as frequency range and equation solver preferences as described in the following procedures.

To 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. Choose one of the following options:

   • Choose Compute real response only if you want Abaqus/Standard to ignore damping terms. This option can significantly reduce computational time.

   • Choose Compute complex response if you want to include damping terms and allow a complex system matrix to be factored.

   For more information, see “Damping” in “Direct-solution steady-state dynamic analysis,” Section 6.3.4 of the Abaqus Analysis User's Guide.

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

5. Toggle on Use eigenfrequencies to subdivide each frequency range if you want the frequency range(s) of interest to be subdivided using the system's eigenfrequencies. This option requires a preceding frequency step. For more information, see “Selecting the type of frequency interval for which output is requested” in “Direct-solution steady-state dynamic analysis,” Section 6.3.4 of the Abaqus Analysis User's Guide.

6. Toggle on Include friction-induced damping effects to include friction-induced contributions to the damping matrix. For more information, see “Contact conditions with sliding friction” in “Direct-solution steady-state dynamic analysis,” Section 6.3.4 of the Abaqus Analysis User's Guide.

7. 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 in the frequency range at which results should be given.

   If you toggled on Use eigenfrequencies to subdivide each frequency range, this is the number of points at which results should be given, 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 you toggled off Use eigenfrequencies to subdivide each frequency range, this is the total number of points in the frequency range, including the end points.

   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. This option is recommended if you have toggled on Use eigenfrequencies to subdivide each frequency range, since the ends of each interval are the eigenfrequencies where the response amplitudes vary most rapidly.

   For more information, see “The bias parameter” in “Direct-solution steady-state dynamic analysis,” Section 6.3.4 of the Abaqus Analysis User's Guide.

   For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.

To configure settings on the Other tabbed page:

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

   (For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

2. Choose a Matrix storage option:

   • Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.

   • Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme.

   • Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.

   For more information on matrix storage, see “Matrix storage and solution scheme in Abaqus/Standard” in “Defining an analysis,” Section 6.1.2 of the Abaqus Analysis User's Guide.

To create or edit a mode-based steady-state dynamic procedure:

1. Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: Linear perturbation; Steady-state dynamics, Modal), or “Editing a step,” Section 14.9.3.

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

To 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. 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. Toggle on Use eigenfrequencies to subdivide each frequency range if you want the frequency range(s) of interest to be subdivided using the system's eigenfrequencies. For more information, see “Selecting the type of frequency interval for which output is requested” in “Mode-based steady-state dynamic analysis,” Section 6.3.8 of the Abaqus Analysis User's Guide.

5. 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 in the frequency range at which results should be given.

   If you toggled on Use eigenfrequencies to subdivide each frequency range, this is the number of points at which results should be given, 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 you toggled off Use eigenfrequencies to subdivide each frequency range, this is the total number of points in the frequency range, including the end points.

   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. This option is recommended if you have toggled on Use eigenfrequencies to subdivide each frequency range, since the ends of each interval are the eigenfrequencies where the response amplitudes vary most rapidly.

   For more information, see “The bias parameter” in “Mode-based steady-state dynamic analysis,” Section 6.3.8 of the Abaqus Analysis User's Guide.

   For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.

To 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,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

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” in “Mode-based steady-state dynamic analysis,” Section 6.3.8 of the Abaqus Analysis User's Guide.

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, , for a particular mode range. 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, .

   • 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, .

        • Beta: stiffness proportional damping, .

   • 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,” Section 3.2.7.

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, , 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, .

   • 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, .

        • Beta: stiffness proportional damping, .

   • 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,” Section 3.2.7.

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

To create or edit a subspace-based steady-state dynamic procedure:

1. Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: Linear perturbation; Steady-state dynamics, Subspace), or “Editing a step,” Section 14.9.3.

2. On the Basic and Other tabbed pages, configure settings such as frequency range and matrix solver preferences as described in the following procedures.

To configure settings on the Basic tabbed page:

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

   (For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

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 one of the following options:

   • Choose Compute real response only if you want Abaqus/Standard to ignore damping terms. This option can reduce computational time.

   • Choose Compute complex response if you want to include damping terms and allow a complex system matrix to be factored.

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

5. Toggle on Include friction-induced damping effects to include friction-induced contributions to the damping matrix. For more information, see “Contact conditions with sliding friction” in “Subspace-based steady-state dynamic analysis,” Section 6.3.9 of the Abaqus Analysis User's Guide.

6. Toggle on Use eigenfrequencies to subdivide each frequency range if you want the frequency range(s) of interest to be subdivided using the system's eigenfrequencies. For more information, see “Selecting the type of frequency interval for which output is requested” in “Subspace-based steady-state dynamic analysis,” Section 6.3.9 of the Abaqus Analysis User's Guide.

7. Click the arrow to the right of the Projection field, and select an option for controlling the frequency of the subspace projections:

   • Select Evaluate at each frequency to project the dynamic equations onto the subspace at each frequency you specify. This method is the most computationally expensive.

   • Select Constant to perform only one projection using model properties evaluated at the center frequency of all ranges and individual frequency points that you specify. This method is the least expensive. However, you should choose this method only when the material properties do not depend strongly on frequency.

   • Select Interpolate at eigenfrequencies to perform the projections at each extracted eigenfrequency in the requested frequency range and at eigenfrequencies immediately outside the range. The projected mass, stiffness, and damping matrices are then interpolated at each frequency point requested.

   • Select As a function of property changes to select how often subspace projections onto the modal subspace are performed based on material property changes as a function of frequency. If you select this option, do the following:

     1. In the Max. damping change field, enter the maximum relative change in damping material properties before a new projection is to be performed.

     2. In the Max. stiffness change field, enter the maximum relative change in stiffness material properties before a new projection is to be performed.

   • Select Interpolate at lower and upper frequency limits to perform projections at the lower and upper limits of the last frequency range. This method can be used only with the SIM architecture.

8. 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 in the frequency range at which results should be given.

   If you toggled on Use eigenfrequencies to subdivide each frequency range, this is the number of points at which results should be given, 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 you toggled off Use eigenfrequencies to subdivide each frequency range, this is the total number of points in the frequency range, including the end points.

   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. This option is recommended if you have toggled on Use eigenfrequencies to subdivide each frequency range, since the ends of each interval are the eigenfrequencies where the response amplitudes vary most rapidly.

   For more information, see “The bias parameter” in “Subspace-based steady-state dynamic analysis,” Section 6.3.9 of the Abaqus Analysis User's Guide.

   For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.

To configure settings on the Other tabbed page:

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

   (For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

2. Choose a Matrix solver option:

   • Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.

   • Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme.

   • Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.

   For more information on matrix storage, see “Matrix storage and solution scheme in Abaqus/Standard” in “Defining an analysis,” Section 6.1.2 of the Abaqus Analysis User's Guide.

To create or edit a substructure generation procedure:

1. Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: Linear perturbation; Substructure generation), or “Editing a step,” Section 14.9.3.

2. On the Basic, Options, and Damping tabbed pages, configure settings such as substructure generation options and damping specifications.

To configure settings on the Basic tabbed page:

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

   (For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

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. In the Substructure identifier field, enter an integer between 1 and 999 that uniquely identifies this substructure in your model. Abaqus prepends a “Z” to the number you specify when it stores the substructure identifier in the model database.

4. If desired, toggle on Evaluate recovery matrix for to enable selective recovery in your analysis, and do one the following:

   • Select Whole model to enable selective recovery for the entire model.

   • Select Region, and select a node set or element set from the list to enable selective recovery for a single set in your model.

To configure settings on the Options tabbed page:

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

   (For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

2. From the Generation Options, do any of the following:

   • Toggle on Compute gravity load vectors to calculate the substructure's gravity load vectors during substructure generation.

   • Toggle on Compute reduced mass matrix to generate a reduced mass matrix for the substructure.

   • Toggle on Compute reduced structural damping matrix to generate a reduced structural damping matrix for the substructure.

   • Toggle on Compute reduced viscous damping matrix to generate a reduced viscous damping matrix for the substructure.

   • Toggle on Evaluate frequency-dependent properties at frequency to evaluate frequency-dependent material properties in substructure generation. If you toggle on this option, you can also specify the custom frequency for the frequency-dependent properties.

3. If you want to specify retained eigenmodes for generation of a coupled acoustic-structural substructure, toggle on Specify retained eigenmodes by, then select either Mode range or Frequency range.

4. If you are specifying retained eigenmodes by mode range, enter the following data in the Data table to generate the list of eigenmodes:

   Start Mode

   The first mode number.

   End Mode

   The end mode number.

   Increment

   The increment in mode numbers between the start and end modes.

   For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.

5. If you are specifying retained eigenmodes by frequency range, 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.

   For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.

To 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,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

2. From the Global Damping Ratios options, specify the Field to which global damping will apply in this step:

   • Choose None to exclude the effects of global damping.

   • Choose All to apply global damping to all of the displacement, rotation, and acoustic fields in a model.

   • Choose Acoustic to apply global damping only to the acoustic fields in a model.

   • Choose Mechanical to apply global damping only to the displacement and rotation fields in a model.

3. If you selected any Field setting other than None, do any of the following:

   • For the Alpha option, specify a value for the first Rayleigh damping ratio.

   • For the Beta option, specify a value for the second Rayleigh damping ratio.

   • For the Structural option, specify a value for the structural damping ratio.

4. From the Viscous damping options, choose one of the following:

   • Choose None to exclude the effects of viscous damping altogether at the usage level.

   • Choose Element to activate only the generated condensed viscous damping matrix of the substructure.

   • Choose Factor to activate only the Rayleigh viscous damping.

   • Choose Combined to activate the combined generated and Rayleigh viscous damping matrix.

5. From the Structural damping options, choose one of the following:

   • Choose None to exclude the structural damping matrix.

   • Choose Element to activate only the generated condensed structural damping matrix of the substructure.

   • Choose Factor to activate only the stiffness proportional structural damping matrix.

   • Choose Combined to activate the combined generated and stiffness proportional.

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

To create or edit a time-harmonic electromagnetic procedure:

1. Display the Edit Step dialog box following the procedure outlined in “Creating a step,” Section 14.9.2 (Procedure type: Linear perturbation; Electromagnetic, Time harmonic), or “Editing a step,” Section 14.9.3.

2. On the Basic and Other tabbed pages, configure settings such as frequency range and equation solver preferences as described in the following procedures.

To 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. 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 in the frequency range at which results should be given. The minimum value is 2. If the value is omitted, the default value of 20 points is assumed.

   For detailed information on how to enter data, see “Entering tabular data,” Section 3.2.7.

To configure settings on the Other tabbed page:

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

   (For information on displaying the Edit Step dialog box, see “Creating a step,” Section 14.9.2, or “Editing a step,” Section 14.9.3.)

2. Choose a Matrix storage option:

   • Choose Use solver default to allow Abaqus/Standard to decide whether a symmetric or unsymmetric matrix storage and solution scheme is needed.

   • Choose Unsymmetric to restrict Abaqus/Standard to the unsymmetric storage and solution scheme.

   • Choose Symmetric to restrict Abaqus/Standard to the symmetric storage and solution scheme.

   For more information on matrix storage, see “Matrix storage and solution scheme in Abaqus/Standard” in “Defining an analysis,” Section 6.1.2 of the Abaqus Analysis User's Guide.