

July 16, 2023 at 12:14 amPuneet ShahareSubscriber
I have a cantilever beam with a vibration envrirnment of :
30g base excitation at 500Hz and 50g at 800 Hz, with linear ramping in between.
How to determine the response of the system for the above conditions? I am interested to know the maximum stresses as well as the life of the structure. 
July 16, 2023 at 2:56 pmpeteroznewmanSubscriber
Take the free courses in Modal analysis and Harmonic Response. Below is a summary of the steps you need to take.
In Workbench, drag a Modal analysis and drop it in the Project Schematic then drag a Harmonic Response and drop it on the Solution cell of the Modal analysis. This creates a Modal Superposition (MSUP) Harmonic Response analysis.
In the Modal analysis, add a Fixed Support to the faces/edges that are connected to the base (ground). Under Modal Analysis Settings, increase the Max Modes to Find to a large number such as 15 modes or higher. Solve the Modal analysis. Click on Solution Information and select Participation Factor Summary for the Solution Output. Scroll down and check the table of Cumulative Effective Mass Fraction. For the X, Y and Z directions, look to see the values have exceeded 0.9 in all three columns before the last mode or increase the number of modes if they have not.
With only 10 modes, you see that the Y direction suddenly goes to 1.0 at Mode 6 without having reached 0.9 first.
Increase the Max number of modes to find to 15 shows a more gradual increase.
With 30 modes, there are plenty of modes with values above 0.9 for the X, Y Z directions.
Another requirement is that the maximum modal frequency in the solution is at least 1.5 times higher than the highest frequency in the acceleration load to be used in the Harmonic Response. We can see that for this model, that requirement is easily met.
In the Harmonic Response branch, add an Acceleration Load. Set the Base Excitation to Yes and in the Tabular Data, enter two rows for 500 and 800 Hz with the correct values of acceleration (converted to m/s^2) and set the correct direction.
Look at the Analysis settings. It is very important to enter a Damping Ratio value to the model. I have used 5%, but you should determine the appropriate value for your structure. Use smaller values to be conservative.
Insert an Equivalent Stress plot and set it to Maximum over Frequency to find the worst stress over the frequency range requested.
Insert another Equivalent Stress plot and set it to Frequency of Maximum to see what frequency has the worst stress.
Finally insert an Equivalent Stress plot and set the frequency to see how the whole structure looks at that worst frequency.
I will post this reply without addressing the Fatigue analysis and the Life prediction. See if you can get your analysis to this point and reply back.

 You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
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.
 Solver Pivot Warning in Beam Element Model
 Saving & sharing of Working project files in .wbpz format
 Understanding Force Convergence Solution Output
 User manual
 An Unknown error occurred during solution. Check the Solver Output…..
 What is the difference between bonded contact region and fixed joint
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 whether have the difference between using contact and target bodies
 Defining rigid body and contact
 Colors and Mesh Display

7780

4504

2971

1449

1322
© 2023 Copyright ANSYS, Inc. All rights reserved.