Running a Random Vibration Analysis
Overview
Random vibration analyses enable you to evaluate how a structure responds to random, frequency-dependent excitations such as the roughness of a road, engine vibration, or turbulent flow. Instead of applying a deterministic load, you define the power spectral density (PSD) of the excitation and study the statistical response of the system.
In Creo Ansys Simulation random vibration analysis is an extension of a modal analysis. You must first define and run a modal analysis. You then apply frequency-dependent PSD loads to the model. The solver uses the model’s natural modes and combines them statistically to predict expected response levels such as deformation, stress, acceleration, or velocity. Results can be scaled using sigma levels that represent the probability of occurrence.
Prerequisites for Running a Random Vibration Analysis
• You must have an advanced Creo Ansys Simulation license to run a random vibration study, or to update results for an existing study.
• The model must be suitable for modal analysis. (Free-free models are not supported). The model must have a least one fixed constraint.
• You must define and run a modal study.
You can specify solver settings that are specific to random vibration analyses.
Running a Random Vibration Analysis
1. Define a modal study or open an existing modal study.
2. Click > and then select the Random Vibration check box to enable random vibration analysis.
 |
Clearing the Random Vibration check box for a previously defined random vibration analysis removes all PSD loads, results, and probes from the study.
|
3. Define at least one fixed constraint for the model. PSD load definition is enabled on the Loads group only after a fixed constraint is defined for the model.
4. Define one or more loads as a function of frequency. Loads must be defined as table functions with variation of the quantity at different frequencies. To define a PSD load perform the following steps:
a. From the Loads group select one of the following loads.
▪ 
PSD Acceleration
PSD Acceleration▪ 
PSD G Acceleration
PSD G Acceleration▪ 
PSD Velocity
PSD Velocity▪ 
PSD Displacement
PSD Displacementb. Right-click the X, Y, or Z component field and select Function to open the Functions dialog box.
| | Load component values cannot have constant values other than 0. They must be only table functions of frequency. |
c. Define a table function with a minimum of two rows, where frequency is the first quantity (X- axis) and the physical quantity (displacement, velocity or acceleration) is the second column (Y—axis) in the table function.
After defining the table function, you can preview the graph using the Graph Function control.
d. Click OK to create the load.
5. Define results for a quantity that you want to study, or define result probes for different result quantities.
6. Click > 
Run to run the random vibration study.
Run to run the random vibration study.7. When the study completes, study global or user-defined results.
Viewing Results
Once the study completes you can view the following global results or define results for the following quantities:
• Deformation
• Acceleration
• Velocity
• Stress
• Elastic strain
• Frequency table
• Reaction forces and moments (probes only)
Selecting Sigma Levels
All results for random vibration studies are probabilistic, represented as sigma levels that allow interpretation of results in terms of likelihood rather than absolute values. Select one of the following values for a result:
• 1 Sigma: approximately 68% probability of occurrence
• 2 Sigma: approximately 95% probability of occurrence
• 3 Sigma: approximately 99.7% probability of occurrence
Random vibration results can be exported to an apr file for reporting or post-processing.
Using Probes
The following type of probes can be defined for results of random vibration studies:
• Value at point
• Maximum, minimum, average, or sum
• Line chart
Defining a Line Chart Probe for Random Vibration Studies
1. Click Simulation Probe on the Ansys Simulation tab.
2. In the Simulation Probe dialog box, select the required Result type.
3. From the Probe type list, select Line Chart.
4. In References, select a single straight line (sketched line or datum curve) on solid geometry.
5. Optionally, enter a positive value in the Scale Factor field.
6. Optionally, enable Reverse direction if you want to reverse the start and end point of the selected reference line.
7. Click OK to create the line chart probe.