November 19, 2023 at 12:07 pmTonmoySubscriber
We are currently working to prescribe some earthquake motions in LS-Dyna (V14.0.0) with LS-PrePost (V4.10.5-23Jun23) and have come across an interesting issue. I'm hoping you can help us with this.
In our simulations model, which involve 6721 nodes and 6244 elements, we prescribed all three components of the ground motions as accelerations. However, when we checked the displacement response of a node from the prescribed motion nodeset from d3plot, there was an unexpected drift at the end of the displacement time-history. Interestingly, this drift doesn't occur if we derive the displacement by integrating the acceleration using alternative methods. This problem happens regardless of the specifics of the input acceleration data, or the target node I choose to compare the integrated acceleration output with the output displacement.
In the figure below, I've plotted the displacement response, integrated from acceleration, alongside the actual displacement response of node 28289 in the x direction with help of the History tool. This is a random node on the surface of the rigid body system subjected to the motion. As you can see, there is a clear difference between the displacement derived by LS-Dyna and the displacement integrated from LS-Dyna's acceleration in LS-PrePost -
Interestingly though, when we approach the problem in reverse – starting with output displacements and then performing differentiation twice to obtain the accelerations of a node – the results align much more closely with the output response acclerations -
I'm trying to understand why this issue happens and if there is something we are doing wrong.
Another question I have is about prescribing ground motions: should we use displacement or acceleration? And how does the internal algorithm of LS-Dyna originally handles this?
Any insights would be greatly appreciated. Thanks in advance for your help!
November 20, 2023 at 9:55 pmUshnish BasuAnsys Employee
Note that any integration or differentiation you do in LSPP or otherwise will be affected by the output timestep. To match LS-DYNA calculations, you should output at the computation timestep and then integrate. Also keep in mind that calculated acceleration is inherently noisy in explicit analysis.
LS-DYNA applies velocities internally, irrespective of whether displacement or acceleration is prescribed, so you can try to apply velocity ground motion records if you have them. Alternatively, you can apply the accelerations using LOAD_BODY if appropriate.
November 20, 2023 at 11:03 pmTonmoySubscriber
Thank you Dr. Basu for your wounderful recommendations.
I have another question in this regard. The LS-Dyna computed time step uses CFL limit, right? So, it changes to smaller or larger value depending on the deformation state of my system at a specific time instance. Should I use the minimum time step to do this comparison then?
November 20, 2023 at 11:26 pmUshnish BasuAnsys Employee
You can specify an output timestep to be very small, e.g. 1e-7, then it will just output at the computation timesteps
November 21, 2023 at 10:39 amTonmoySubscriber
I really appreciate your help and guidance to resolve this issue. The application of intertia force through LOAD_BODY worked like a charm and solved the problem. I also tried out the small timestep suggestion and now I can overlay LS-Dyna calculated displacement with alternatives.
Thank you again for your time and all the suggestions.
- The topic ‘LS-Dyna result: displacement vs acceleration’ is closed to new replies.
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.
- Maximum Time Step
- Error 20211 (STR+211) while 2D impact analysis
- ls dyna has no solver
- LS-Dyna Prestressed
- Whereabouts of the LS-DYNA program manager
- License error : NO SUITABLE FEATURE FOUND
- Total Contact Force and Contact Pressure
- Contact not working in Ls-Dyna and Ls-Dyna ACT (WB)
- Element direction..
- TIED_CONTACT for Shell Elements – Gap between Shell-Shell and Shell-Solid
© 2023 Copyright ANSYS, Inc. All rights reserved.