www.kxcad.net Home > CAE Index > ANSYS Index > Release 11.0 Documentation for ANSYS Workbench

This analysis enables you to determine the response of structures to vibration loads that are random in nature. An example would be the response of a sensitive electronic component mounted in a car subjected to the vibration from the engine, pavement roughness, and acoustic pressure.

Loads such as the acceleration caused by the pavement roughness are not deterministic, that is, the time history of the load is unique every time the car runs over the same stretch of road. Hence it is not possible to predict precisely the value of the load at a point in its time history. Such load histories, however, can be characterized statistically (mean, root mean square, standard deviation). Also random loads are non-periodic and contain a multitude of frequencies. The frequency content of the time history is captured (spectrum) along with the statistics and used as the load in the random vibration analysis. This spectrum, for historical reasons, is called Power Spectral Density or PSD.

In a random vibration analysis since the input excitations are statistical in nature, so are the output responses such as displacements, stresses, and so on.

Typical applications include aerospace and electronic packaging components subject to engine vibration, turbulence and acoustic pressures, tall buildings under wind load, structures subject to earthquakes, and ocean wave loading on offshore structures.

The excitation(s) is applied in the form of Power Spectral Density (PSD). The PSD is a table of spectral values vs. frequency that captures the frequency content. The PSD captures the frequency and mean square amplitude content of the load’s time history.

The square root of the area under a PSD curve represents the root mean square (rms) value of the excitation. The unit of the spectral value of acceleration, for example, is G

^{2}/Hertz.The input excitation is expected to be stationary (the average mean square value does not change with time) with a zero mean.

This analysis is based on the mode superposition method. Hence a modal analysis that extracts the natural frequencies and mode shapes is a prerequisite.

This feature covers one type of PSD excitation only- base excitation.

The base excitation could be an acceleration PSD (either in acceleration

^{2}units or in G^{2}units), velocity PSD or displacement PSD.The base excitation is applied in the specified direction to all entities that have a Fixed Support boundary condition. Other support points in a structure such as

**Frictionless Surface**are not excited by the PSD.Multiple uncorrelated PSDs can be applied. This is useful if different, simultaneous excitations occur in different directions.

If stress/strain results are of interest from the random vibration analysis then you will need to request stress/strain calculations in the modal analysis itself. Only displacement results are available by default.

Postprocessing:

The results output by the solver are one sigma or one standard deviation values (with zero mean value). These results follow a Gaussian distribution. The interpretation is that 68.3% of the time the response will be less than the standard deviation value.

You can scale the result by 2 times to get the 2 sigma values. The response will be less than the 2 sigma values 95.91% of the time and 3 sigma values 99.737% of the time.

Since the directional results from the solver are statistical in nature they cannot be combined in the usual way. For example the X, Y, and Z displacements cannot be combined to get the magnitude of the total displacement. The same holds true for other derived quantities such as principal stresses.

A special algorithm by Segalman-Reese is used to compute a meaningful value for equivalent stress.

**Attach Geometry**

*Basic
general information about this topic*

**...
for this analysis type:**

There are no specific considerations for a random vibration analysis.

**Define Part Behavior**

*Basic
general information about this topic*

**...
for this analysis type:**

Both Young’s modulus (or stiffness in some form) and density (or mass in some form) must be defined in the modal analysis. Material properties must be linear but can be isotropic or orthotropic, and constant or temperature-dependent. Nonlinear properties, if any, are ignored.

**Define Connections**

*Basic
general information about this topic*

**...
for this analysis type:**

Only linear behavior is valid in a random vibration analysis. Nonlinear elements, if any, are treated as linear. If you include contact elements, for example, their stiffnesses are calculated based on their initial status and are never changed.

Joints are not allowed in a random vibration analysis.

Only the stiffness of springs are taken into account in a random vibration analysis.

**Apply Mesh Controls/Preview Mesh**

*Basic
general information about this topic*

**...
for this analysis type:**

There are no specific considerations for a random vibration analysis.

**Define Analysis Type**

*Basic
general information about this topic*

**...
for this analysis type:**

Choose

Random Vibrationas theNew Analysistype.

**Establish Analysis Settings**

*Basic
general information about this topic*

**...
for this analysis type:**

For a random vibration analysis the basic controls are:

Options for Modal, Harmonic, Linear Buckling, and Random Vibration Analyses. The only applicable option is to specify the number of modes to use from the modal analysis. A conservative rule of thumb is to include modes that cover 1.5 times the maximum frequency in the PSD excitation table.

Damping Controls allow you to specify damping for the structure in the random vibration analysis. Alpha and Beta damping as well as constant damping ratio are available for a random vibration analysis. In addition material dependent damping can also be applied using the Engineering Data module.

Analysis Data Management settings enable you to save solution files from the

Random Vibrationanalysis. The default behavior is to only keep the files required for postprocessing. You can use these controls to keep all files created during solution or to create and save an ANSYS database (db file).

**Define Initial Condition**

*Basic
general information about this topic*

**...
for this analysis type:**

You must point to a modal analysis in the

Initial Conditionenvironment field. The modal analysis must extract enough modes to cover the PSD frequency range. A conservative rule of thumb is to extract enough modes to cover 1.5 times the maximum frequency in the PSD excitation.

**Apply Loads and Supports**

*Basic
general information about this topic*

**...
for this analysis type:**

Any support boundary condition must be defined in the modal analysis itself. You cannot add any new support boundary conditions in the random vibration analysis.

The only applicable load is a

PSD Base Excitationof spectral value vs. frequency.All Fixed Supports in the modal analysis are excited by all of the PSD excitation tables in the given direction.

The PSD table is defined and stored in Engineering Data module. You can create a new PSD table or import one from a library via the fly-out in the Details View of the

PSD Base Excitationload.Four types of base excitation are supported:

PSD Acceleration,PSD G Acceleration,PSD Velocity, andPSD Displacement.Each PSD base excitation should be given a direction in global Cartesian system.

Multiple PSD excitations (uncorrelated) can be applied. Typical usage is to apply 3 different PSDs in the X, Y, and Z directions. Correlation between PSD excitations is not supported.

**Solve**

*Basic
general information about this topic*

**...
for this analysis type:**

Solution Informationcontinuously updates any listing output from the solver and provides valuable information on the behavior of the structure during the analysis. In addition to solution progress you will also find the participation factors for each PSD excitation. The solver output also has a list of the relative importance of each mode in the modal covariance matrix listing.

**Review Results**

*Basic
general information about this topic*

**...
for this analysis type:**

If stress/strain results are of interest from the random vibration analysis then you will need to request stress/strain calculations in the modal analysis itself. You can use the

Output ControlsunderAnalysis Settingsin the modal analysis for this purpose. Only displacement results are available by default.Applicable results are Directional (X/Y/Z) Displacement/Velocity/Acceleration, normal and shear stresses/strains and equivalent stress. These results can be displayed as contour plots.

The displacement results are relative to the base of the structure (the fixed supports).

The velocity and acceleration results include base motion effects (absolute).

Since the directional results from the solver are statistical in nature they cannot be combined in the usual way. For example the X, Y, and Z displacements cannot be combined to get the magnitude of the total displacement. The same holds true for other derived quantities such as principal stresses.

By default the 1 σ results are displayed. You can apply a scale factor to review any multiples of σ such as 2 σ or 3 σ. The Details View as well as the legend for contour results also reflects the percentage (using Gaussian distribution) of time the response is expected to be below the displayed values.

Meaningful equivalent stress is computed using a special algorithm by Segalman-Reese. Note that the probability distribution for this equivalent stress is neither Gaussian nor is the mean value zero. However, the “3 σ” rule (multiplying the RMS value by 3) yields a conservative estimate on the upper bound of the equivalent stress.

**Create Report (optional)**

*Basic
general information about this topic*

**...
for this analysis type:**

There are no specific considerations for a random vibration analysis.

The following example illustrates performing a random vibration analysis in Simulation.

Open the model in Simulation, establish units, and set up a random vibration analysis.

Open the file

`BoardWithChips.dsdb`from one of the following locations:Windows platform:

`...\Program Files\ANSYS Inc\v110\AISOL\Samples\Simulation`Unix platform:

`.../ansys_inc/v110/aisol/Samples/Simulation`

From the main menu, choose

**Units> U. S. Customary (in, lbm, lbf,**^{o}**F, s, V, A**).Choose

**New Analysis> Map of Analysis Types...**, click on the**Random Vibration**box then on**OK**.This automatically creates a

**Modal**analysis as an initial condition to the**Random Vibration**analysis.If you already have a modal analysis in the tree, you can link it as the initial condition by choosing the modal analysis name in the

**Initial Condition Environment**drop down list.

Apply fixed supports and any other support boundary conditions in the modal analysis. Only “fixed” supports are excited by the PSD in the random vibration analysis.

Highlight the

**Fixed Support**object, then select the inner faces of the two holes. In the Details View, click in the**Geometry**field, then click on the**Apply**button.

Solve the modal analysis then review the mode shapes and get a feel for the behavior of the structure.

See step 2, and steps 4 through 8 in the Example: Modal Analysis. After choosing

**Solve**, an error message may appear stating that you need at least one structural load to proceed with the solution. This has no effect on the modal analysis so you can proceed with the next step in the example.

Request as many modes as required in the modal analysis. The highest frequency mode should be about 1.5 times the highest frequency value expected in the PSD curve.

Add a PSD Base Excitation load. This is the only load allowed in the random vibration analysis.

Under the

**Random Vibration**analysis environment object, choose**Loads> PSD Base Excitation**from the toolbar.Use the fly-out menu to add a new PSD load and choose

**PSD G Acceleration**as the type of PSD excitation.You can also create a library of PSD curves and import one from the library.

Define the PSD curve in Engineering Data.

Click

**OK**after choosing the PSD type to automatically move to Engineering Data.Click on

**PSD G Acceleration vs. Frequency**in the tree and enter values in the table to build the PSD curve.

Specify the direction of the PSD excitation. All fixed supports specified in the modal analysis will get excited by the PSD excitation.

Click on the

**Simulation**tab to return to Simulation.Set

**Direction**to**Z Axis**.

Solve the random vibration analysis.

Choose

**Solve**from the toolbar.The

**Solution Information**worksheet shows important information about modes that were included in solution.

Specify result types.

Highlight the

**Solution**object under**Random Vibration**and choose the following result types from the toolbar:**Stress> Equivalent (von Mises)****Deformation> Directional Velocity**In the Details View, set

**Orientation**to**Z Axis**.

**Deformation> Directional**In the Details View, set

**Orientation**to**Z Axis**.**Deformation> Directional Acceleration**In the Details View, set

**Orientation**to**Z Axis**.

Highlight all result items, click the right mouse button and choose

**Rename Based on Definition**.

Evaluate result types.

Highlight the

**Solution**object under**Random Vibration**, click the right mouse button and choose**Evaluate All Results**.

Review results.

Click on any result item and note the Details View information and the result graphic.

Notes on random vibration results:

Directional Deformation, velocity, and acceleration quantities are available for review.

Velocity and acceleration results are absolute while deformation is relative to the fixed supports.

You can specify the scale factor on the results to get 1, 2, or 3 sigma results.

Equivalent stress is computed using Segalman-Reese algorithm which yields a conservative estimate on the upper bound of the equivalent stress.