ProductsAbaqus/StandardAbaqus/CAE IntroductionSteady-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 direct-solution steady-state dynamic procedure conducts this frequency sweep. In a direct-solution steady-state analysis the steady-state harmonic response is calculated directly in terms of the physical degrees of freedom of the model using the mass, damping, and stiffness matrices of the system. When defining a direct-solution 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. Those 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 (described below). The direct-solution steady-state analysis procedure can be used in the following cases for which the eigenvalues cannot be extracted (and, thus, the mode-based steady-state dynamics procedures are not applicable):
While the response in this procedure is linear, the prior response can be nonlinear. Initial stress effects (stress stiffening) as well as load stiffness effects will be included in the steady-state dynamics response if nonlinear geometric effects (General and perturbation procedures) were included in any general analysis step prior to the direct-solution steady-state dynamic procedure. Input File Usage STEADY STATE DYNAMICS, DIRECT Abaqus/CAE Usage Step module: Create Step: Linear perturbation: Steady-state dynamics, Direct Ignoring dampingIf damping terms can be ignored, you can specify that a real, rather than a complex, system matrix be factored, which can significantly reduce computational time. Damping is discussed below. Input File Usage STEADY STATE DYNAMICS, DIRECT, REAL ONLY Abaqus/CAE Usage Step module: Create Step: Linear perturbation: Steady-state dynamics, Direct: Compute real response only Selecting the type of frequency interval for which output is requestedThree types of frequency intervals are permitted for output from a direct-solution steady-state dynamic step. If an eigenvalue extraction step precedes the direct-solution steady-state dynamic step, you can select either the range or the eigenfrequency type of frequency interval; otherwise, only the range type can be used. Dividing the specified frequency range using the user-defined number of points and the optional bias functionFor the range type of frequency interval (the default), the specified frequency range of interest is divided using the user-defined number of points and the optional bias function. Input File Usage STEADY STATE DYNAMICS, DIRECT, INTERVAL=RANGE Abaqus/CAE Usage Step module: Create Step: Linear perturbation: Steady-state dynamics, Direct: toggle off Use eigenfrequencies to subdivide each frequency range Specifying the frequency ranges by using the system's eigenfrequenciesIf the direct-solution steady-state dynamic analysis is preceded by an eigenfrequency extraction step, you can select the eigenfrequency type of frequency interval. The following intervals then exist in each frequency range:
For each of these intervals the frequencies at which results are calculated are determined using the user-defined number of points (which includes the bounding frequencies for the interval) and the optional bias function. Figure 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, DIRECT, INTERVAL=EIGENFREQUENCY Abaqus/CAE Usage Step module: Create Step: Linear perturbation: Steady-state dynamics, Direct: Use eigenfrequencies to subdivide each frequency range Figure 1. Division of range for the eigenfrequency type of interval and 5
calculation points.
Specifying the frequency ranges by the frequency spreadIf the direct-solution steady-state dynamic analysis is preceded by an eigenfrequency extraction step, you can select the spread type of frequency interval. In this case 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 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. Figure 2. Division of range for the spread type of interval and 5 calculation
points.
and
are eigenfrequencies of the system.
Input File Usage STEADY STATE DYNAMICS, DIRECT, 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. Selecting the frequency spacingTwo types of frequency spacing are permitted for a direct-solution 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, DIRECT, FREQUENCY SCALE=LOGARITHMIC STEADY STATE DYNAMICS, DIRECT, FREQUENCY SCALE=LINEAR Abaqus/CAE Usage Step module: Create Step: Linear perturbation: Steady-state dynamics, Direct: Scale: Logarithmic or Linear Requesting multiple frequency rangesYou can request multiple frequency ranges or multiple single frequency points for a direct-solution steady-state dynamic step. Input File Usage STEADY STATE DYNAMICS, DIRECT 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, Direct: Data: enter data in table, and add rows as necessary The bias parameterThe 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 3 shows a few examples of the effect of the bias parameter on the frequency spacing. Figure 3. Effect of the bias parameter on the frequency spacing for a number of
points .
The bias formula used in direct-solution steady-state dynamics is where
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 1.0 for a range frequency interval and 3.0 for an eigenfrequency interval. The frequency scale factorThe 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). DampingIf 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. In direct-solution steady-state dynamics damping can be created by the following:
When a real-only system matrix is factored, all forms of damping are ignored, including quiet boundaries on infinite elements and nonreflecting boundaries on acoustic elements. Contact conditions with sliding frictionAbaqus/Standard automatically detects the contact nodes that are slipping due to velocity differences imposed by the motion of the reference frame or the transport velocity in prior steps. At those nodes the tangential degrees of freedom are not constrained and the effect of friction results in an unsymmetric contribution to the stiffness matrix. At other contact nodes the tangential degrees of freedom are constrained. Friction at contact nodes at which a velocity differential is imposed can give rise to damping terms. There are two kinds of friction-induced damping effects. The first effect is caused by the friction forces stabilizing the vibrations in the direction perpendicular to the slip direction. This effect exists only in three-dimensional analysis. The second effect is caused by a velocity-dependent friction coefficient. If the friction coefficient decreases with velocity (which is usually the case), the effect is destabilizing and is also known as “negative damping.” For more details, see Coulomb friction. Direct-solution steady-state dynamics analysis allows you to include these friction-induced contributions to the damping matrix. Input File Usage STEADY STATE DYNAMICS, DIRECT, FRICTION DAMPING=YES Abaqus/CAE Usage Step module: Create Step: Linear perturbation: Steady-state dynamics, Direct: Include friction-induced damping effects Initial conditionsThe 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). Initial condition definitions that directly define solution variables, such as velocity, cannot be used in a steady-state dynamic analysis. Boundary conditionsIn a steady-state dynamic analysis the real and imaginary parts of any degree of freedom are either restrained or unrestrained simultaneously; 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 prescribed specifically. The unspecified part will be assumed to have a perturbation magnitude of zero. Boundary conditions can be applied to any of the displacement or rotation degrees of freedom (1–6) in a direct-solution steady-state analysis. See Boundary conditions in Abaqus/Standard and Abaqus/Explicit. These boundary conditions will vary sinusoidally with time. You specify the real (in-phase) part of a boundary condition and the imaginary (out-of-phase) part of a boundary condition separately. Input File Usage Use either of the following options to define the real (in-phase) part of the boundary condition: BOUNDARY BOUNDARY, REAL Use the following option to define the imaginary (out-of-phase) part of the boundary condition: BOUNDARY, IMAGINARY Abaqus/CAE Usage Load module: boundary condition editor: real (in-phase) part + imaginary (out-of-phase) parti Frequency-dependent boundary conditionsAn amplitude definition can be used to specify the amplitude of a boundary condition as a function of frequency (Amplitude Curves). Input File Usage Use both of the following options: AMPLITUDE, NAME=name BOUNDARY, REAL or IMAGINARY, AMPLITUDE=name Abaqus/CAE Usage Load or Interaction module: Create Amplitude: Name:name Load module: boundary condition editor: real (in-phase) part + imaginary (out-of-phase) parti: Amplitude:name LoadsThe following loads can be prescribed in a steady-state dynamic analysis:
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. Coriolis distributed loading adds an imaginary antisymmetric contribution to the overall system of equations. This contribution is currently accounted for in solid and truss elements only and is activated by using the unsymmetric matrix storage and solution scheme for the step (Defining an analysis). Incident wave loads can be used to model sound waves from distinct planar or spherical sources or from diffuse fields. Fluid flux loading cannot be used in a steady-state dynamic analysis. Input File Usage Use any of the following options to define the real (in-phase) part of the load: CLOAD or DLOAD CLOAD or DLOAD, REAL Use either of the following options 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) parti Frequency-dependent loadingAn amplitude definition can be used to specify the amplitude of a load as a function of frequency (Amplitude Curves). 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) parti: Amplitude:name Predefined fieldsPredefined temperature fields can be specified in direct-solution steady-state dynamic analysis (see Predefined Fields) and will produce harmonically varying thermal strains if thermal expansion is included in the material definition (Thermal expansion). Other predefined fields are ignored. Material optionsAs in any dynamic analysis procedure, mass or density (Density) must be assigned to some regions of any separate parts of the model where dynamic response is required. If an analysis is desired in which the inertia effects are neglected, the density should be set to a very small number. The following material properties are not active during steady-state dynamic analyses: plasticity and other inelastic effects, thermal properties (except for thermal expansion), mass diffusion properties, electrical properties (except for the electrical potential, , in piezoelectric analysis), and pore fluid flow properties—see General and perturbation procedures. Viscoelastic effects can be included in direct-solution steady-state harmonic response analysis. The linearized viscoelastic response is considered to be a perturbation about a nonlinear preloaded state, which is computed on the basis of purely elastic behavior (long-term response) in the viscoelastic components. Therefore, the vibration amplitude must be sufficiently small so that the material response in the dynamic phase of the problem can be treated as a linear perturbation about the predeformed state. Viscoelastic frequency domain response is described in Frequency domain viscoelasticity. ElementsAny of the following elements available in Abaqus/Standard can be used in a steady-state dynamic procedure:
OutputIn direct-solution steady-state dynamic analysis the value of an output variable such as strain (E) or stress (S) is a complex number with real and imaginary components. In the case of data file output the first printed line gives the real components while the second lists the imaginary components. Results and data file output variables are also provided to obtain the magnitude and phase of many variables (see Abaqus/Standard output variable identifiers). In the case of data file output the first printed line gives the magnitudes while the second lists the phase angle. The following variables are provided specifically for steady-state dynamic analysis: Element integration point variables:
For connector elements, the following element output variables are available:
Nodal variables:
The total kinetic energy of an element (ELKE) is not available for output in a direct-solution steady-state dynamic analysis. The elastic strain energy density (SENER) is not available for output in a SIM-based steady-state dynamic analysis. Whole model variables such as ALLIE (total strain energy) are available for direct-solution steady-state dynamic analysis by requesting energy output to the data, results, or output database files (see Output to the Data and Results Files and Output to the Output Database). Input file templateHEADING … AMPLITUDE, NAME=loadamp Data lines to define an amplitude curve as a function of frequency (cycles/time) ** STEP, NLGEOM Include the NLGEOM parameter so that stress stiffening effects will be included in the steady-state dynamic step STATIC **Any general analysis procedure can be used to preload the structure … CLOAD and/or DLOAD Data lines to prescribe preloads TEMPERATURE and/or FIELD Data lines to define values of predefined fields for preloading the structure BOUNDARY Data lines to specify boundary conditions to preload the structure … END STEP ** STEP STEADY STATE DYNAMICS, DIRECT Data lines to specify frequency ranges and bias parameters BOUNDARY, REAL Data lines to specify real (in-phase) boundary conditions BOUNDARY, IMAGINARY Data lines to specify imaginary (out-of-phase) boundary conditions CLOAD, AMPLITUDE=loadamp Data lines to specify sinusoidally varying, frequency-dependent, concentrated loads CLOAD and/or DLOAD Data lines to specify sinusoidally varying loads … END STEP |