Inserting a New Subspace-based Steady-State Dynamics Step
Inserting a subspace-based steady-state dynamic analysis step within the Simulation History enables you to calculate the steady-state dynamic linearized response of a system to harmonic excitation. This type of procedure is based on direct solution of the steady-state dynamic equations projected onto a subspace of modes. Abaqus calculates the response based on the system's eigenfrequencies and modes, which must first be extracted by using the eigenfrequency extraction procedure in a Frequency step.
Subspace-based steady-state dynamic steps are available only in a Nonlinear Structural case. They can be defined in new cases or in cases that contain other general static or static linear perturbation steps. Subspace-based steady-state dynamic steps cannot be defined in an Explicit Dynamics case or in a Thermal case. See Step Sequence Restrictions for more information.
This task shows you how to insert a new Subspace-based Steady-State Dynamic step in a Nonlinear Structural case.
Select Start>Analysis & Simulation>Nonlinear Structural Analysis from the menu bar to enter the Nonlinear Structural Analysis workbench.
From the New Analysis Case dialog box, select Nonlinear Structural Case.
Click the Steady-State Dynamics Step: Subspace icon
.Tip: Alternatively, you can select Insert>Steady-State Dynamics Step: Subspace from the menu bar, or you can right-click the last step in the simulation history and select Insert Step Below>Steady-State Dynamics Step: Subspace from the menu that appears.
The Steady-State Dynamics Step: Subspace dialog box appears, and a Steady State Dynamics Step: Subspace Step objects set appears in the specification tree under the Simulation History objects set for the current Nonlinear Structural case.
You can change the step identifier by editing the Step name field. This name will be used in the specification tree.
Enter a description for the step in the Step description field.
Choose a Frequency scale option to indicate whether you want the frequency range(s) of interest to be divided using a Logarithmic or Linear scale.
From the Interval options, do one of the following:
Select Eigenfrequency to subdivide the frequency range(s) of interest using the system's eigenfrequencies.
Select Range to subdivide the frequency range(s) of interest using the number of points you specify in the Frequency sampling data table.
Enter the following data in the Frequency sampling 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 selected Eigenfrequency as the sampling Interval, this value 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 selected Range as the sampling Interval, this value 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 four 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 selected Eigenfrequency as the sampling Interval, since the ends of each interval are the eigenfrequencies where the response amplitudes vary most rapidly.
If you want to provide global damping values, do the following:
Toggle on Use global damping data.
Enter any of the following values:
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.
From the Type of response selections, choose one of the following options:
Choose Real if you want Abaqus to ignore damping terms. This option can reduce computational time.
Choose Complex if you want to include damping terms and allow a complex system matrix to be factored.
Toggle on Include friction-induced damping to include friction-induced contributions to the damping matrix.
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 eigenfrequency 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:
In the Max. damping change field, enter the maximum relative change in damping material properties before a new projection is to be performed.
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. You should select this option only when SIM architecture has been selected in the preceding frequency step.
Click OK when you have finished defining the step.
The Steady-State Dynamics Step (Subspace) objects set contains a default Field Output Request object in a Field Output Requests objects set. See Requesting Results for more information.