Revision History

Note

All SolidPractices are written as guidelines. It is a strong recommendation to use these documents only after properly evaluating your requirements. Distribution of this document is limited to Dassault Systèmes SolidWorks employees, VARs, and customers that are on active subscription. You may not post this document on blogs or any internal or external forums without prior written authorization from Dassault Systèmes SolidWorks Corporation.

This document was updated using version SOLIDWORKS 2022 SP05. If you have questions or need assistance in understanding the content, please get in touch with your designated reseller.

Preface

Linear dynamic studies are useful for determining a structure’s response to both deterministic and nondeterministic time-dependent loading. This is accomplished by solving the structural matrix equation of motion \$\left\lbrack \text{M} \right\rbrack\left\{ \ddot{\text{u}} \right\}\text{+}\left\lbrack \text{C} \right\rbrack\left\{ \dot{\text{u}} \right\}\text{+}\left\lbrack \text{K} \right\rbrack\left\{ \text{u} \right\}\text{=\{}\text{F}\left( \text{t} \right)\text{\}}\$ using modal analysis, which can allow for fast and efficient solutions. The computational efficiency and accuracy are heavily based on the modes of the system’s natural frequencies that are used when approximating the solution. This SolidPractice provides an introduction to linear dynamic analysis, its applications, and the best practices for achieving accurate results.

Students reading this document should be familiar with the SOLIDWORKS Simulation software, and the principles of linear static analysis, and modal frequency analysis.

Your Feedback Requested

We would like to hear your feedback and suggestions for new topics. After reviewing this document, please take a few minutes to fill out a brief survey. Your feedback will help us create the content that directly addresses your challenges.

Introduction

When performing a linear dynamic study, as with all types of SOLIDWORKS Simulation studies, it is important to understand what types of situations you should consider, and how a linear dynamic study differs from other study types.

Static studies use the assumption that all loads are constant or applied very slowly, neglecting any inertial or damping forces. In cases where loads change with time or frequency, you should use a dynamic study instead. When a structure encounters a time varying load, its response is based on its natural mode shapes. The SOLIDWORKS Simulation software does not account for these frequencies and mode shapes when performing any type of static study.

To analyze such responses, linear dynamic studies run based on the normal mode method. The study first calculates the natural frequencies and mode shapes of the structure. The study then determines the response of each mode that is based on the applied loading, and uses that response to calculate the combined response of the model.

When to Perform a Dynamic Analysis

Consider performing a dynamic type of analysis when:

• Transient responses are necessary.
• Inertial forces and damping are a significant factor.
• The load/excitation frequencies are close to the structure’s natural frequency.

\$\$\frac{\text{First fundamental frequency of the structure}}{\text{Largest frequency of the applied loads}}\text{≤3}\$\$

Linear Dynamic vs. Nonlinear Dynamic

The SOLIDWORKS Simulation software can to perform both linear dynamic studies, and nonlinear dynamic studies. Linear dynamic studies make the following assumptions:

• All materials behave linearly according to Hooke’s Law.
• The calculated response is limited to linear small displacements based on a constant stiffness matrix.
• All deformations are elastic, allowing recovery of the structure’s original shape upon removal of the loading. There is no residual stress or strain in the structure.
• Contact interaction (no penetration contact) conditions are not allowed.

Accordingly, if you need to simulate large displacements, contact behavior, advanced material models (Von Mises Plasticity, hyperelasticity, etc.), or need to solve the fully coupled equation of motion, the recommendation is that you instead create a nonlinear type of study.

Steps in a Linear Dynamic Analysis

The general steps to perform a linear dynamic study are:

1. Determine the type of loading and the associated frequencies. This is important in determining the type of linear dynamic analysis to use, and to determine how to set the analysis up.
2. Run a natural frequency analysis and evaluate the structural modes. Linear dynamic studies have a built-in frequency study. The linear dynamic study results are based on the data derived from this frequency analysis.
3. Compare the load frequencies to that of the structure to determine if they fall within similar ranges.
   • If the normal mode frequencies are well outside the range of load frequencies, then a dynamic analysis might not be required.
   • If the normal mode frequencies are within the range of load frequencies, then the recommendation is to run a dynamic analysis.

Frequency Analysis

A frequency analysis is performed before running a linear dynamic analysis to determine the natural modes of the structure. This analysis provides the shape and frequency of the free vibration modes, and the mass participation factor based on the modes analyzed.

Because these modes are the basis for the linear dynamic study, it is important that these results are accurate. You want to make sure that any factors that can affect your model’s natural modes are accurately accounted for, including (but not limited to):

• The model geometry
• Boundary conditions (fixtures)
• Material properties (stiffness)
• Mesh quality and accuracy
• Additional masses, springs, and connections within the study

Resonance

When the frequency of the exciting force coincides with a natural frequency of the structure, resonant vibrations could eventually lead to failure. Examples of this type of failure include troops marching across a bridge, or the voice of an opera singer breaking glass.

While resonance may lead to failure in some cases, in other cases resonance may be intentional. Some objects function based on the principle of resonance, such as a tuning fork.

Mass Participation Factor

In many scenarios, it is mainly the lower frequencies that dominate the response of a structure, with higher frequencies being ignored. However, to get a better measure of the frequencies that you might need to consider in an analysis, you can use the mass participation factor.

The mass participation factor in a frequency analysis is the expected contribution of each frequency mode to the kinetic energy of the structure in a particular direction. The total participating mass in the direction of motion is equal to the total participating mass of the structure.

In general, a ratio of 80% in each of the three directions is indicative of a reasonable solution accuracy. In addition to the number of modes included in the frequency analysis, the mass participation will also depend on factors such as:

• The model geometry
• The components materials
• The connections between components
• The interactions between components
• How the model is restrained

This mass participation factor is used to approximate the adequate number of modes to include in the dynamic analysis. A higher value is better than a lower value. However, an 80% value does not necessarily guarantee that all important modes are included. You must be sure that the mesh is fine enough to properly discretize the model, and that the mass in regions of interest adequately participates in the included frequency modes.

In some cases, depending on the restraints or geometry, a value of 80% might be impossible to reach. For example, if the analysis includes base or ground components, the base plate may be much stiffer and heavily restrained than the other components. Often, base components may even be fully fixed. This would result in high natural frequencies which may be difficult to resolve and would typically fall outside the frequency range of interest.

If such a base component contributes significantly to the overall mass of the analysis model and its associated modes are not important, then you can expect a mass participation lower than 80%, even with all important modes included. If you are unsure if this is the case, you may run tests that exclude base components and replace them with appropriate fixtures. This type of test can provide a sense of how much the base components affect the overall mass participation.

It is also a good practice to re-run the analysis with a finer mesh and higher number of modes to verify that the results are converged.

Dynamic Analysis Concepts

Linear dynamic analysis is based on the structural equation of motion given by:

[C] = damping matrix \$\text{\{}\dot{\text{u}}\text{\}}\$ = nodal velocity

[K] = stiffness matrix {u} = nodal displacement

{F(t)} = time-dependent force

In a static analysis, the inertial and damping terms would be ignoring. However, in a dynamic analysis, these terms remain included in the solution.

Dynamic analysis can analyze time-dependent loads that are deterministic or nondeterministic. The result is the response vs. time/frequency, or global peak values. There is more information about the results of each type of dynamic analysis later in this document.

Characteristics of Dynamic Behavior

A dynamic response involving deformation is normally oscillatory in nature, in which the structure vibrates about a stable equilibrium configuration. The total response of a structure using this type of analysis is approximated by the modal superposition method. Therefore, it is important that all modes that contribute to the deformation shape of the structure are considered in the analysis. Figure 1 shows a case in that should include at least five modes to characterize the deformation shape.

Damping

Damping characterizes the energy dissipation from a structure. This can occur through a variety of phenomena, making it a difficult factor to model exactly. Three of the major sources of damping are:

• Frictional effects between components. Any components in contact with each other have some degree of frictional interaction. As components in contact vibrate, frictional forces acting against the movement consume some of the energy.
• Material damping that occurs at the molecular level due to material deformations and reorientations. Examples of this are plastic deformations of the material, and reorientations of ferromagnetic vectors.
• Viscous damping, which accounts for energy dissipative effects as the vibrating structure displaces the surrounding fluid. The viscous damping magnitude is given by:

Fd=c∙vn

Fd=damping force v=structural velocity

c=damping magnitude n=exponent (typically 1)

Figure 2 shows an example of the physical causes of damping in a building structure.

In a damped system, there is a critical damping value at which the system converges to zero in the minimum amount of time. If the system is underdamped, the system will oscillate with decreasing amplitude before returning to zero. Overdamped systems will not exhibit oscillations, but takes longer than the optimal time to return to zero. Figure 3 depicts that in both the underdamped and overdamped cases, the system takes longer to reach equilibrium than the critically damped system.

The SOLIDWORKS software supports two types of damping: Rayleigh damping and modal damping. For Rayleigh damping, the damping matrix is a proportional combination of the mass and stiffness matrices where:

[C]=α[M]+β[K]

[C]=damping matrix [M] = mass matrix [K] = stiffness matrix

A user inputs values for α and β, then SOLIDWORKS calculates the damping ratio for each frequency mode. If you want to dampen higher frequencies, use an α close to 0 and a β close to 1. To dampen lower frequencies, use an α close to 1 and a β close to 0.

The values of α and β can come from correlating analysis results with test data, or from civil engineering building codes such as the Uniform Building Code (UBC) and the International Building Code (IBC). The internet has other good sources for α and β values.

The modal damping ratio (MDR) method is generally a more direct and convenient method than using Rayleigh damping. MDR defines the modal damping as a percentage of the critical damping. For each frequency mode, you would specify a damping ratio. For example, in civil engineering building codes, if a frequency is below 5 Hz a damping less than 2% is used, while a 5% damping is used for frequencies of 5-20 Hz. Damping ratios typically range from 0.01 for lightly damped systems to 0.15 or more for highly damped systems.

For material-specific damping, you can define a composite modal damping ratio as a material property (MDAMP). In this way, you can assign different damping ratios for different parts. SOLIDWORKS uses these ratios internally to calculate an equivalent modal damping ratio for each mode. Some typical values include:

• Metals within elastic range: < 0.01
• Aluminum/Steel transmission lines: ≈ 0.0004
• Small diameter piping systems: 0.01-0.02
• Automobile shock absorbers: ≈0.30
• Rubber: ≈0.05
• Large buildings during earthquakes: 0.01-0.05
• Prestressed concrete structures: 0.02-0.05
• Reinforced concrete structures: 0.04-0.07
• See the SOLIDWORKS Online Help topic “Viscous Damping Ratios”

Modal Time History Analysis

Modal time history studies determine the response of structures based on known (deterministic) time-dependent loads and excitations such as:

• Shock (pulsed) loads
• General periodic or nonperiodic time-varying loads
• Base excitation motions (displacement, velocity, or acceleration applied to all or selected supports)
• Initial displacement, velocity, or acceleration conditions

The results of a modal time history analysis are also given as a function of time. The value chosen for the time step is critical to obtaining valid results. Unlike a nonlinear dynamic study where you might pick autostepping, the time step here must be constant. As a general guideline, consider the following criteria when choosing the time step:

• The time resolution of the highest important modal wave. Optimally, it is important to discretize the modal wave by at least 10 time steps (5 minimum).

Dt=0.1 Tmin

Dt = Maximum time step size

Tmin = Period of the highest important vibration mode

• The time resolution of the loading. Because loads are time-dependent, it is important to capture all significant wave characteristics in the time steps.

Dt=0.1 Tload

Dt = Maximum time step size

Tload = Characteristic time of the load (duration of shock, period of oscillation, etc.)

• The resolution of the shock wave propagation (optional). When investigating a transient response, there are times when the stress wave that travels through a structure is important when investigating its response (such as an impact test). In this case, you need to resolve this shock wave based on its speed and distance of travel.

\$\$\text{D}_{\text{t}}\text{= }\frac{\text{0.2 }\text{L}_{\text{characteristic}}}{\text{v}_{\text{elastic wave}}}\text{= }\frac{\text{0.2 }\text{L}_{\text{characteristic}}}{\sqrt{\frac{\text{E}}{\text{ρ}}}}\$\$

Dt = Maximum time step size

Lcharacteristic = Characteristic length of the model (length along which the shock wave propagates)

velastic wave = Speed of sound in the material

E = Young’s Modulus of Elasticity

ρ = Mass density

Harmonic Analysis

Harmonic studies determine the response of structures due to harmonic forces or base excitations over a range of frequencies. Unlike modal time history analysis, which evaluates a transient response with time of a loading condition, harmonic analysis solves for the steady-state peak response at different operational frequencies. For example, the amplitude and phase response of a system due to applied harmonic forces or excitations.

Both the excitation and response are functions of frequency, rather than time. The results depend only on the number of modes included, and not on the frequency size step. The excitations can have amplitudes that vary with respect to frequency. The response gives the maximum nodal response (acceleration, velocity, and displacement) and phase. Because the excitation is harmonic, the response is also harmonic and has the same frequencies.

• Response at each frequency is due to the excitation at that frequency only.
• All loads must be sinusoidal and have the same frequency. If multiple load functions are used, they may have different amplitude and phase.
• Modal damping is supported.
• Transient effects are not taken into account.

• Harmonic analysis allows for fast computation of amplitude response for a range of frequencies.

Both the modal time history and the harmonic analysis studies can evaluate harmonic types of loading; however, each uses a different method.

• Harmonic loading in time history analysis:
  • Sine waves with or without exponential rise or decay
  • Deterministic with respect to the start and end time
  • Elaborates the transient aspect of a signal
  • Solution for the given fixed frequencies in the equation
  • Possible to apply loads at different locations with varying frequencies to see the combined effect

• Harmonic analysis:

  • No exponential rise or decay
  • Steady-state with an infinite time period
  • No transient effects due to initial conditions
  • Provides response for a wide range of frequencies
  • Response at each frequency is due to the excitation at the same time frequency only
  • No simultaneous excitations with different frequencies
  • Fast computation of amplitude of response

Random Vibration Analysis

Random vibration studies determine the response of structures due to random (nondeterministic) excitations described by power spectral density (PSD) functions versus frequency. This study type can represent loads such as:

• Base accelerations generated by earthquakes
• Loads generated on a car wheel traveling on a rough road
• Pressure generated by air turbulence
• Pressure from sea waves or strong wind

The analysis calculates the root mean square (RMS) and PSD response to the PSD excitations.

Power Spectral Density (PSD) Functions

The random loading for the vibration analysis is represented by a PSD function. The PSD function represents the vibrational frequencies and energy in a statistical form. PSD units may be in units of:

• \$\frac{\left\lbrack \text{Force} \right\rbrack^{\text{2}}}{\text{frequency}}\$
• \$\frac{\left\lbrack \text{Displacement} \right\rbrack^{\text{2}}}{\text{frequency}}\$
• \$\frac{\left\lbrack \text{Velocity} \right\rbrack^{\text{2}}}{\text{frequency}}\$
• \$\frac{\left\lbrack \text{Acceleration} \right\rbrack^{\text{2}}}{\text{frequency}}\$

Examples of PSD levels (over 25-250 Hz) include:

• 0.001 g2/Hz as in a passenger airplane
• 0.01 g2/Hz most electronic equipment tested
• 0.1 g2/Hz feels uncomfortable, military equipment
• 1 g2/Hz intolerable

Random processes are often identified by the shape of their PSD functions.

Figure 4: Example of random processes in time and frequency Domain

	F(t)	PSD(ω)
Sinusoidal
Narrow-Band
Wide-Band
Ideal White Noise

Random Vibration Options

When setting up a random vibration study, in addition to determining the number of modes to include in the analysis, you must also define the operating frequency limits within the Random Vibration Options tab of the study properties.

The options within the Random Vibration Options tab allow you to set the exciting frequency range that the solution considers in its analysis by setting the lower limit and upper limit frequencies. For example, if the exciting frequencies extend above the default Upper limit frequency value, you must manually input an appropriate value that will cover the range of frequencies to consider in the analysis.

Within the Random Vibration Options and its Advanced Options tab you can also adjust options which set determine the number of frequency points to be selected between adjacent natural frequencies, as well as the biasing parameter which controls the selection of frequency points for integration.

You can find more detailed information about these options as well as others in the Online Help articles “Random Vibration” and “Random Vibration – Advanced.”

Response Spectrum Analysis

Response spectrum analysis studies determine the maximum response of a structural given a specified input spectrum. This study can simulate problems with random or shock base excitations. The input is a response spectrum that provides the maximum response of a single degree of freedom (DOF) system vs. natural frequency. The output is the overall peak response due to the input excitation. Although the excitation is a function of frequency, this output response is neither a function of frequency nor time.

The input is a curve of maximum responses of single DOF systems of different natural frequencies to the same base motion. In practice, you would start with the transient acceleration loading as shown in Figure 5. This excitation would be applied onto a single degree of freedom oscillator that has some mass and stiffness that we know the natural frequency for. The peak response of this system is measured, which makes one data point for the response spectrum. This is repeated so that the peak response is plotted for a range of single degree of freedom systems so that you have the peak response as a function of natural frequency. An example single DOF system response to an excitation is shown in Figure 5.

Damping effects are taken into account in the input response spectrum by incorporating damping effects into the single DOF systems themselves. Different spectrum curves are usually available for different values of modal damping ratio of the single DOF system. Otherwise, it is customary to use a damping ratio of 5%, which is the normal damping ratio of most buildings.

To determine the overall peak response, the contributions from the max responses of the individual modes must be combined. The SOLIDWORKS software offers four different mode combination methods:

• Square Root Sum of Squares (SRSS). This method takes the square root of the sum of the squares of the maximum responses.
• Absolute Sum. This method assumes that the maximum response of all individual modes occurs at the same time. The peak response is therefore the summation of all maximum responses, making it the most conservative method.
• Complete Quadratic Combination (CQC). This method is based on random vibration theory. It is thought to be an improvement on the SRSS method for closely spaced modes.
• Navy Research Laboratory (NRL). This method takes the absolute value of the response for the mode with the largest response, then adds it to the SRSS response of the remaining modes.

For more information about each of these methods, see the topic “Mode Combination Techniques” in the SOLIDWORKS Online Help.

Other General Tips

• Choosing the number of modes:
  • Solution accuracy depends heavily on the number of natural modes considered.
  • In dynamic problems under the influence of base excitations, usually the number of modes considered must contribute to a total mass participation factor of at least 80% of the system mass in the direction of the base motion.
  • For harmonic and random vibration problems, in addition to the 80% mass participation factor requirement, the range of natural frequencies considered for analysis must cover the highest frequency in the excitation.
  • In the case of systems under the influence of force excitations, it is essential to consider all modes that contribute to the static deformation shape of the structure.
  • These are simply guidelines, and do not guarantee the inclusion of all important modes. Carefully analyze the problem setup and obtained results to determine if all important modes have been considered.
• Dead loads, gravity, etc. in a time history study:
  • Perform a static analysis with this load. Go to the dynamic studies properties, and activate the Dead load effects option.
• Accurate fixtures and boundary conditions:
  • Fixtures, boundary conditions, and model simplifications can heavily affect the natural modes of a structure. This in turn can alter the linear dynamic results significantly. Therefore, it is important to accurately model the setup as closely to reality as possible.
• Contact conditions:
  • Only Bonded interaction and Free interaction conditions are available for linear dynamic studies.
• Why are bolts and contacts not supported in linear dynamic studies?
  • Bolt connectors and contacts introduce nonlinearities that require additional calculations a linear dynamic study does not support.
• Meshing considerations:
  • Because the analysis results are heavily dependent on the system’s natural modes, it is important to have a mesh that is adequately refined. Meshes that are too coarse might fail to smoothly capture mode shapes, stiffen the model enough to significantly alter the frequency values, or eliminate some mode shapes altogether in extreme cases.
  • Always observe the deformed shape of the highest mode to see if it looks smooth and well characterized. It is also a recommendation to perform a convergence test by remeshing and solving with a higher mesh density, and then comparing natural mode results to see if they are significantly affected by the mesh refinement.
• Result options for linear dynamic studies:
  • Before running an analysis, review and modify the result options as needed in the Result Options PropertyManager.
  • In the Result Options PropertyManager, you can specify to save results For all solution steps, or For specified solution steps. Before running an analysis with a large number of solution steps, determine whether you require results from all steps or only a specific range of steps. Saving a large number of solution steps can require a large amount of disk space, particularly for models meshed with many elements.
  • When you interpret the displacement and velocity results, it is important to consider whether the results use Relative or Absolute quantities. This option is located in the Result Options PropertyManager for linear dynamic studies.
    • With the Relative option, displacement and velocity quantities are output relative to the base movement defined by a Uniform Base Excitation.
    • With the Absolute option, the displacement and velocity quantities are given in absolute values. This is the case if you apply Selected Base Excitation loads.
  • If no result locations are specified for the Locations for graphs option, results at all nodes are saved. This can lead to very large results files.

We hope that you find this document informational and useful and request that you leave a brief feedback about the topics that you want us to cover in the next revision of this document. Click here for a complete list of SolidPractices documents available from DS SOLIDWORKS Corp.