March 16, 2018 at 9:41 pmmomidorSubscriber
I have the worst case combination of accelerations and I'm curious how apply this to the simple beam fatigue Ansys simulations.
Acceleration factors [·m/s2]
March 16, 2018 at 10:19 pmpeteroznewmanSubscriber
I'm not sure what the "simple beam fatigue Ansys simulations" are, but I know a bit about fatigue and vibrations.
Fatigue is due to cycles of stress amplitude. More cycles creates more fatigue damage, and higher amplitudes creates more fatigue damage.
You have provided an amplitude, but no frequency information. Are these amplitudes at a specific frequency? You also need to provide a duration this vibration is applied to determine the fatigue damage. Longer duration creates more fatigue damage.
When I test samples for fatigue on a single-axis shaker table, and I have a specification for x, y and z directions, I apply the vibrations sequentially on each axis. The damage is accumulated through the three tests as the vibration is applied in the three directions in sequential tests.
March 17, 2018 at 10:01 ammomidorSubscriber
I would like to apply let say 10 kN vertical only concentrate force which is acting on the edge of beam. This beam is suppose to be working for 10 years under accelerations ax,ay,az which is acting with frequency 1/8 Hz. Should I use the Random Vibration module ? Actually it's not random but rather very steady.
March 17, 2018 at 2:22 pmpeteroznewmanSubscriber
What is creating the 10 kN force at the tip? If it is a spring or cable to the sea floor, then you can apply a force, but if it is a 1,020 kg mass at the end of the beam, you should add that concentrated mass at the end of the beam and turn on gravity to deflect the beam. The mass needs to be present when the base accelerations occur.
Add a Static Structural system feeding into a Modal system so you get the effect of the 10kN prestress, then feed that into three Harmonic Response systems to find out the peak response to harmonic base vibrations in the range 0.0625 (1/16) to 0.25 (1/4) Hz to account for the some uncertainty around the 1/8 Hz frequency.
You can then request a frequency response. Here is the Z axis tip displacement of 0.545 mm at 1/8 Hz with the 10 kN tip force.
If I suppress the 10 kN force and add a 1020 kg mass to the tip, then the response in Z is much larger at 5.3 mm
March 18, 2018 at 12:40 ampeteroznewmanSubscriber
Importance of Damping in Dynamic Analysis
I don't know the length and beam properties of your example, but in the example I made up, I used higher frequencies to see the different modes that are in my structure. I do this to show that the peak response is highly dependent on the damping in the model. For lightly damped structures, you also have to refine the frequency spacing so as not to cut off the peak with a poor choice of frequencies in the result.
In the first plot I requested a linear spacing of 200 points between 0 and 100 Hz and I see there are two peaks with the maximum stress of 186.9 MPa, but if I request a log spacing of 200 points, then the peak stress jumps to 705 MPa, so the first plot misses the peak. But this is unrealistic because there is no damping.
In the third plot, I keep the log spacing but add 0.1 Constant Damping to the model and the peak stress is now 111.3 MPa and that won't change much with a tighter spacing of frequencies in the result plot.
With acceleration at the higher frequencies, the fatigue tool begins to show a finite life on the steel material.
Life shows 200,000 cycles to failure, and at 8 seconds/cycle, that means failure is predicted to occur in 1.6 million seconds or 444 hours or 18.5 days for my made-up example.
- 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.
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.
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- 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
- A solver pivot warning or error has been detected
© 2023 Copyright ANSYS, Inc. All rights reserved.