

July 5, 2021 at 4:23 pmAutonewbieSubscriber
Hi, after reading some notes... I still not able to determine when to use response spectrum or random vib. Anyone can share your tips? Thanks!

July 5, 2021 at 5:35 pmpeteroznewmanSubscriberLook at the input data you have to excite the structure.
If the input is a table of values of acceleration PSD values in the units of G^2/Hz vs frequency in Hz, that is the type of input you use in a Random Vibration analysis. The output of the Random Vibration analysis is the 1sigma value of stress, which means the response will be less than that value 68% of the time. You can multiply that value of stress by a factor of 2 to get a 2sigma value and the response will be less than that value 95.45% of the time. You can multiply that value of stress by a factor of 3 to get a 3sigma value and the response will be less than that value 99.73% of the time.
If the input is a table of values of acceleration in units of G vs frequency in Hz, that is the type of input you use in a Response Spectrum analysis. The output of the Response Spectrum analysis is the predicted maximum response the structure will have to that input.
The above examples mention acceleration, but tables using velocity or displacement are also possible, though less common.
Both Random Vibe and Response Spectrum have in common a requirement for a Modal Analysis with a Fixed Support to create the Base Excitation where the input goes in.
If you have accelerationtime data, and not a short table of values vs frequency, you can compute either a PSD table or a Shock Response Spectrum table to use as input.
If the accelerationtime data is a sample from a vibration source that may run for a long time, like an engine, and each time you record a sample of the vibration using an accelerometer, the statistical values of the recording are the same, then you would want to analyze a structure subject to that vibration using Random Vibration.
If the accelerationtime data is the complete record of an event, such as an earthquake, and you want to know if the structure will survive that particular event, then you want to analyze the structure using Response Spectrum.
Read the help to learn more. Open ANSYS Help from the Start menu, then copy paste the URL below into the address bar.
https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v211/en/wb_sim/ds_response_spectrum_analysis_type.html
https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v211/en/wb_sim/ds_spectral_analysis_type.html
If you have accelerationtime data, you could use that data directly as input to a Transient Structural analysis, but for even small models, the computational time to run a 30 second earthquake can be long and it is much faster to convert the accelerationtime data into a Shock Response Spectrum and run the Response Spectrum analysis.
If instead of an event like an earthquake, which has a specific maximum acceleration, you record acceleration data from a running engine, generating random vibrations. Because of the statistical nature of the vibration, the longer you record, the larger the maximum acceleration will be. You can predict the probability of exceeding a specific value by doing statistics on a relatively short recording, even if that value was not recorded.
When I have accelerationtime data, I use a matlab script called vibrationdata to create a PSD table or a Shock Response Spectrum table for input into ANSYS.

 You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from lifesaving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
 How to calculate the residual stress on a coating by Vickers indentation?
 An Unknown error occurred during solution. Check the Solver Output…..
 Saving & sharing of Working project files in .wbpz format
 Solver Pivot Warning in Beam Element Model
 Understanding Force Convergence Solution Output
 Colors and Mesh Display
 whether have the difference between using contact and target bodies
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 Massive amount of memory (RAM) required for solve
 What is the difference between bonded contact region and fixed joint

1970

1730

945

726

397
© 2022 Copyright ANSYS, Inc. All rights reserved.