김경종
23 KiB
6.3.8 MODE-BASED STEADY-STATE DYNAMIC ANALYSIS
Products: Abaqus/Standard Abaqus/CAE
References
• “Defining an analysis,” Section 6.1.2
• “General and linear perturbation procedures,” Section 6.1.3
• “Dynamic analysis procedures: overview,” Section 6.3.1
• “Direct-solution steady-state dynamic analysis,” Section 6.3.4
• “Natural frequency extraction,” Section 6.3.5
• “Subspace-based steady-state dynamic analysis,” Section 6.3.9
• *STEADY STATE DYNAMICS
• “Configuring a mode-based steady-state dynamic analysis” in “Configuring linear perturbation analysis procedures,” Section 14.11.2 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
Overview
A mode-based steady-state dynamic analysis:
• is used to calculate the steady-state dynamic linearized response of a system to harmonic excitation;
• is a linear perturbation procedure;
• calculates the response based on the system’s eigenfrequencies and modes;
• requires that an eigenfrequency extraction procedure be performed prior to the steady-state dynamic analysis;
• can use the high-performance SIM software architecture (see “Using the SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1);
• can include nondiagonal damping effects (i.e., from material or element damping) only when using the SIM architecture;
• is an alternative to direct-solution steady-state dynamic analysis, in which the system’s response is calculated in terms of the physical degrees of freedom of the model;
• can include computation of acoustic contribution factors to help determine the major contributors to acoustic noise;
• is computationally cheaper than direct-solution or subspace-based steady-state dynamics;
• is less accurate than direct-solution or subspace-based steady-state analysis, in particular if significant material damping is present, and
• is able to bias the excitation frequencies toward the values that generate a response peak.
Introduction
Steady-state dynamic analysis provides the steady-state amplitude and phase of the response of a system due to harmonic excitation at a given frequency. Usually such analysis is done as a frequency sweep by applying the loading at a series of different frequencies and recording the response; in Abaqus/Standard the steady-state dynamic analysis procedure is used to conduct the frequency sweep.
In a mode-based steady-state dynamic analysis the response is based on modal superposition techniques; the modes of the system must first be extracted using the eigenfrequency extraction procedure. The modes will include eigenmodes and, if activated in the eigenfrequency extraction step, residual modes. The number of modes extracted must be sufficient to model the dynamic response of the system adequately, which is a matter of judgment on your part.
When defining a mode-based steady-state dynamic step, you specify the frequency ranges of interest and the number of frequencies at which results are required in each range (including the bounding frequencies of the range). In addition, you can specify the type of frequency spacing (linear or logarithmic) to be used, as described below (“Selecting the frequency spacing”). Logarithmic frequency spacing is the default. Frequencies are given in cycles/time.
These frequency points for which results are required can be spaced equally along the frequency axis (on a linear or a logarithmic scale), or they can be biased toward the ends of the user-defined frequency range by introducing a bias parameter (see “The bias parameter,” below).
While the response in this procedure is for linear vibrations, the prior response can be nonlinear. Initial stress effects (stress stiffening) will be included in the steady-state dynamics response if nonlinear geometric effects (“General and linear perturbation procedures,” Section 6.1.3) were included in any general analysis step prior to the eigenfrequency extraction step preceding the steady-state dynamic procedure.
Input File Usage: *STEADY STATE DYNAMICS
The DIRECT and SUBSPACE PROJECTION parameters must be omitted from the *STEADY STATE DYNAMICS option to conduct a mode-based steady-state dynamic analysis.
Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Modal
Selecting the type of frequency interval for which output is requested
Three types of frequency intervals are permitted for output from a mode-based steady-state dynamic step.
Specifying the frequency ranges by using the system’s eigenfrequencies
By default, the eigenfrequency type of frequency interval is used; in this case the following intervals exist in each frequency range:
• First interval: extends from the lower limit of the frequency range given to the first eigenfrequency in the range.
• Intermediate intervals: extend from eigenfrequency to eigenfrequency.
• Last interval: extends from the highest eigenfrequency in the range to the upper limit of the frequency range.
For each of these intervals the frequencies at which results are calculated are determined using the userdefined number of points (which includes the bounding frequencies for the interval) and the optional bias function (which is discussed below and allows the sampling points on the frequency scale to be spaced closer together at eigenfrequencies in the frequency range). Thus, detailed definition of the response close to resonance frequencies is allowed. Figure 6.3.8–1 illustrates the division of the frequency range for 5 calculation points and a bias parameter equal to 1.
Input File Usage: *STEADY STATE DYNAMICS, INTERVAL=EIGENFREQUENCY
Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Modal: Use eigenfrequencies to subdivide each frequency range
flowchart
graph TD
A["frequency points"] --> B["lower end of the range"]
A --> C["mode n"]
A --> D["mode n +1"]
A --> E["mode n + 2"]
A --> F["upper end of the range"]
Figure 6.3.8–1 Division of range for the eigenfrequency type of interval and 5 calculation points.
Specifying the frequency ranges by the frequency spread
If the spread type of frequency interval is selected, intervals exist around each eigenfrequency in the frequency range. For each of the intervals the equally spaced frequencies at which results are calculated are determined using the user-defined number of points (which includes the bounding frequencies for the interval). The minimum number of frequency points is 3. If the user-defined value is less than 3 (or omitted), the default value of 3 points is assumed. Figure 6.3.8–2 illustrates the division of the frequency range for 5 calculation points.
The bias parameter is not supported with the spread type of frequency interval.
Input File Usage: *STEADY STATE DYNAMICS, INTERVAL=SPREAD lwr_freq, upr_freq, numpts, bias_param, freq_scale_factor, spread
Abaqus/CAE Usage: You cannot specify frequency ranges by frequency spread in Abaqus/CAE.
text_image
Frequency points (1 - spread) · fₙ (1 + spread) · fₙ Frequency points (1 - spread) · fₙ₊₁ (1 + spread) · fₙ₊₁ fₙ₊₁
Figure 6.3.8–2 Division of range for the spread type of interval and 5 calculation points. f _ { n } and f _ { n + 1 } are eigenfrequencies of the system.
Specifying the frequency ranges directly
If the alternative range type of frequency interval is chosen, there is only one interval in the specified frequency range spanning from the lower to the upper limit of the range. This interval is divided using the user-defined number of points and the optional bias function, which can be used to space the sampling frequency points closer to the range limits. For the range type of frequency interval, the peak responses around the system’s eigenfrequencies may be missed since the sampling frequencies at which output will be reported will not be biased toward the eigenfrequencies.
Input File Usage: *STEADY STATE DYNAMICS, INTERVAL=RANGE
Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Modal: toggle off Use eigenfrequencies to subdivide each frequency range
Selecting the frequency spacing
Two types of frequency spacing are permitted for a mode-based steady-state dynamic step. For the logarithmic frequency spacing (the default), the specified frequency ranges of interest are divided using a logarithmic scale. Alternatively, a linear frequency spacing can be used if a linear scale is desired.
Input File Usage: Use either of the following options:
*STEADY STATE DYNAMICS, FREQUENCY SCALE=LOGARITHMIC
*STEADY STATE DYNAMICS, FREQUENCY SCALE=LINEAR
Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Modal: Scale: Logarithmic or Linear
Requesting multiple frequency ranges
You can request multiple frequency ranges or multiple single frequency points for a mode-based steadystate dynamic step.
Input File Usage: *STEADY STATE DYNAMICS lwr_freq1, upr_freq1, numpts1, bias_param1, freq_scale_factor1 lwr_freq2, upr_freq2, numpts2, bias_param2, freq_scale_factor2 ... single_freq1 single_freq2 ... Repeat the data lines as often as necessary. Abaqus/CAE Usage: Step module: Create Step: Linear perturbation: Steady-state dynamics, Modal: Data: enter data in table, and add rows as necessary
The bias parameter
The bias parameter can be used to provide closer spacing of the results points either toward the middle or toward the ends of each frequency interval. Figure 6.3.8–3 shows a few examples of the effect of the bias parameter on the frequency spacing.
flowchart
graph TD
A["frequency points"] --> B["1"]
A --> C["2"]
A --> D["3"]
A --> E["4"]
A --> F["5"]
style A fill:#f9f,stroke:#333
style B fill:#ccf,stroke:#333
style C fill:#ccf,stroke:#333
style D fill:#ccf,stroke:#333
style E fill:#ccf,stroke:#333
style F fill:#ccf,stroke:#333
Figure 6.3.8–3 Effect of the bias parameter on the frequency spacing for a number of points .
The bias formula used to calculate the frequency at which results are presented is as follows:
\hat {f} _ {k} = \frac {1}{2} (\hat {f} _ {1} + \hat {f} _ {2}) + \frac {1}{2} (\hat {f} _ {2} - \hat {f} _ {1}) | y | ^ {1 / p} \mathrm{sign} (y),
where
y = -1+2(k - 1)/(n- 1);
n is the number of frequency points at which results are to be given within a frequency interval (discussed above);
k is one such frequency point (k = 1, 2, \ldots, n) ; \hat{f}_{1} is the lower limit of the frequency interval; \hat{f}_{2} is the upper limit of the frequency interval; \hat{f}_{k} is the frequency at which the kth results are given;
p is the bias parameter value; and \hat{f} is the frequency or the logarithm of the frequency, depending on the value used for the frequency scale parameter.
A bias parameter, p, that is greater than 1.0 provides closer spacing of the results points toward the ends of the frequency interval, while values of p that are less than 1.0 provide closer spacing toward the middle of the frequency interval. The default bias parameter is 3.0 for an eigenfrequency interval and 1.0 for a range frequency interval.
The frequency scale factor
The frequency scale factor can be used to scale frequency points. All the frequency points, except the lower and upper limit of the frequency range, are multiplied by this factor. This scale factor can be used only when the frequency interval is specified by using the system’s eigenfrequencies (see “Specifying the frequency ranges by using the system’s eigenfrequencies,” above).
Selecting the modes and specifying damping
You can select the modes to be used in modal superposition and specify damping values for all selected modes.
Selecting the modes
You can select modes by specifying the mode numbers individually, by requesting that Abaqus/Standard generate the mode numbers automatically, or by requesting the modes that belong to specified frequency ranges. If you do not select the modes, all modes extracted in the prior eigenfrequency extraction step, including residual modes if they were activated, are used in the modal superposition.
Input File Usage: Use one of the following options to select the modes by specifying mode numbers: *SELECT EIGENMODES, DEFINITION=MODE NUMBERS *SELECT EIGENMODES, GENERATE, DEFINITION=MODE NUMBERS Use the following option to select the modes by specifying a frequency range: *SELECT EIGENMODES, DEFINITION=FREQUENCY RANGE
Abaqus/CAE Usage: You cannot select the modes in Abaqus/CAE; all modes extracted are used in the modal superposition.
Specifying modal damping
Damping is almost always specified for a steady-state analysis (see “Material damping,” Section 26.1.1). If damping is absent, the response of a structure will be unbounded if the forcing frequency is equal
to an eigenfrequency of the structure. To get quantitatively accurate results, especially near natural frequencies, accurate specification of damping properties is essential. The various damping options available are discussed in “Material damping,” Section 26.1.1. You can define a damping coefficient for all or some of the modes used in the response calculation. The damping coefficient can be given for a specified mode number or for a specified frequency range. When damping is defined by specifying a frequency range, the damping coefficient for a mode is interpolated linearly between the specified frequencies. The frequency range can be discontinuous; the average damping value will be applied for an eigenfrequency at a discontinuity. The damping coefficients are assumed to be constant outside the range of specified frequencies.
Input File Usage: Use the following option to define damping by specifying mode numbers:
* \mathrm { M O D A L \ D A M P I N G } , \mathrm { D E F I N I T I O N = M O D E \ N U M B E R S }
Use the following option to define damping by specifying a frequency range:
* \mathrm { M O D A L \ D A M P I N G } , \mathrm { D E F I N I T I O N = F R E Q U E N C Y \ R A N G E }
Use the following option to define damping by global factors:
Abaqus/CAE Usage: Use the following input to define damping by specifying mode numbers:
Step module: Create Step: Linear perturbation:
Steady-state dynamics, Modal: Damping
Defining damping by specifying frequency ranges is not supported in Abaqus/CAE.
Example of specifying damping
Figure 6.3.8–4 illustrates how the damping coefficients at different eigenfrequencies are determined for the following input:
*MODAL DAMPING, DEFINITION=FREQUENCY RANGE
f _ { 1 } , d _ { 1 }
f _ { 2 } , d _ { 2 }
f _ { 2 } , d _ { 3 }
f _ { 3 } , d _ { 3 }
f _ { 4 } , d _ { 4 }
Rules for selecting modes and specifying damping coefficients
The following rules apply for selecting modes and specifying modal damping coefficients:
• No modal damping is included by default.
• Mode selection and modal damping must be specified in the same way, using either mode numbers or a frequency range.
• If you do not select any modes, all modes extracted in the prior frequency analysis, including residual modes if they were activated, will be used in the superposition.
• If you do not specify damping coefficients for modes that you have selected, zero damping values will be used for these modes.
line
| frequency | damping values |
|---|---|
| f₁ | d₁ |
| λ₁ | d₂ |
| f₂ | d₃ |
| f₃ | d₄ |
| f₄ | d₄ |
| λ₃ | d₄ |
Figure 6.3.8–4 Damping values specified by frequency range.
• Damping is applied only to the modes that are selected.
• Damping coefficients for selected modes that are beyond the specified frequency range are constant and equal to the damping coefficient specified for the first or the last frequency (depending which one is closer). This is consistent with the way Abaqus interprets amplitude definitions.
Specifying global damping
For convenience you can specify constant global damping factors for all selected eigenmodes for mass and stiffness proportional viscous factors, as well as stiffness proportional structural damping. For further details, see “Damping in dynamic analysis” in “Dynamic analysis procedures: overview,” Section 6.3.1.
Input File Usage: *GLOBAL DAMPING, ALPHA=factor, BETA=factor, STRUCTURAL=factor
Abaqus/CAE Usage: Defining damping by global factors is not supported in Abaqus/CAE.
Material damping
Structural and viscous material damping (see “Material damping,” Section 26.1.1) is taken into account in a SIM-based steady-state dynamic analysis. Since the projection of damping onto the mode shapes is performed only one time during the frequency extraction step, significant performance advantages can be achieved by using the SIM-based steady-state dynamic procedure (see “Using the SIM architecture for modal superposition dynamic analyses” in “Dynamic analysis procedures: overview,” Section 6.3.1).
If the damping operators depend on frequency, they will be evaluated at the frequency specified for property evaluation during the frequency extraction procedure.
You can deactivate the structural or viscous damping in a mode-based steady-state dynamic procedure if desired.
| Input File Usage: | Use the following option to deactivate structural and viscous damping in a specific steady-state dynamic step:*DAMPING CONTROLS, STRUCTURAL=NONE, VISCOUS=NONE |
| Abaqus/CAE Usage: | Damping controls are not supported in Abaqus/CAE. |
Initial conditions
The base state is the current state of the model at the end of the last general analysis step prior to the steady-state dynamic step. If the first step of an analysis is a perturbation step, the base state is determined from the initial conditions (“Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1). Initial condition definitions that directly define solution variables, such as velocity, cannot be used in a steady-state dynamic analysis.
Boundary conditions
In a mode-based steady-state dynamic analysis both the real and imaginary parts of any degree of freedom are either restrained or unrestrained; it is physically impossible to have one part restrained and the other part unrestrained. Abaqus/Standard will automatically restrain both the real and imaginary parts of a degree of freedom even if only one part is restrained.
Base motion
It is not possible to prescribe nonzero displacements and rotations directly as boundary conditions (“Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.3.1) in mode-based dynamic response procedures. Therefore, in a mode-based steady-state dynamic analysis, the motion of nodes can be specified only as base motion; nonzero displacement or acceleration history definitions given as boundary conditions are ignored, and any changes in the support conditions from the eigenfrequency extraction step are flagged as errors. The method for prescribing base motion in modal superposition procedures is described in “Transient modal dynamic analysis,” Section 6.3.7.
Base motions can be defined by a displacement, a velocity, or an acceleration history. For an acoustic pressure the displacement is used to describe an acoustic pressure history. If the prescribed excitation record is given in the form of a displacement or velocity history, Abaqus/Standard differentiates it to obtain the acceleration history. The default is to give an acceleration history for mechanical degrees of freedom and to give a displacement for an acoustic pressure.
When secondary bases are used, low frequency eigenmodes will be extracted for each “big” mass applied in the model. Use care when choosing the frequency lower limit range in such cases. The “big” mass modes are important in the modal superposition; however, the response at zero or arbitrarily low frequency level should not be requested since it forces Abaqus/Standard to calculate responses at frequencies between these “big” mass eigenfrequencies, which is not desirable.
Frequency-dependent base motion
An amplitude definition can be used to specify the amplitude of a base motion as a function of frequency (“Amplitude curves,” Section 34.1.2).
| Input File Usage: | Use both of the following options: |
| *AMPLITUDE, NAME=name | |
| *BASE MOTION, REAL or IMAGINARY, AMPLITUDE=name |
| Abaqus/CAE Usage: | Load module; Create Boundary Condition; Step: step_name; Category: Mechanical; Types for Selected Step: Displacement base motion or Velocity base motion or Acceleration base motion; Basic tabbed page: Degree-of-freedom: U1, U2, U3, UR1, UR2, or UR3; Amplitude: name |
Loads
The following loads can be prescribed in a mode-based steady-state dynamic analysis, as described in “Concentrated loads,” Section 34.4.2:
• Concentrated nodal forces can be applied to the displacement degrees of freedom (1–6).
• Distributed pressure forces or body forces can be applied; the distributed load types available with particular elements are described in Part VI, “Elements.”
These loads are assumed to vary sinusoidally with time over a user-specified range of frequencies. Loads are given in terms of their real and imaginary components.
Fluid flux loading cannot be used in a steady-state dynamic analysis.
Input File Usage: Use either of the following input lines to define the real (in-phase) part of the load:
*CLOAD or *DLOAD *CLOAD or *DLOAD, REAL
Use the following input line to define the imaginary (out-of-phase) part of the load:
*CLOAD or *DLOAD, IMAGINARY
Abaqus/CAE Usage: Load module: load editor: real (in-phase) part + imaginary (out-of-phase) part i
Frequency-dependent loading
An amplitude definition can be used to specify the amplitude of a load as a function of frequency (“Amplitude curves,” Section 34.1.2).
| Input File Usage: | Use both of the following options: |
| *AMPLITUDE, NAME=name | |
| *CLOAD or *DLOAD, REAL or IMAGINARY, AMPLITUDE=name |
| Abaqus/CAE Usage: | Load or Interaction module: Create Amplitude: Name: name |
| Load module: load editor: real (in-phase) part + imaginary (out-of-phase) | |
| part i: Amplitude: name |