

June 4, 2023 at 5:56 amWooMin JangSubscriber
Hi i wanna do slope stability analysis in LSDYNA.
But there's a problem with gravity initialization.
Dynamic Relaxation or Implicit initialization both give geometries that is not same with slope i modelled...
Is there any way to initialize gravity with "original geometry " to be undeformed...
Because it is slope stability analysis, it is essential to apply gravity load...
Thanks in advance.
P.S.Upper is original(h=20m) and Down is after DR(Initialziation)(h=17.xxm)

June 5, 2023 at 2:30 pmJim DayAnsys EmployeeUse the results you already have to estimate an initial geometry that, when settled due to gravity, gives you close to the geometry you want. You can iterate using this approach a couple of times to get the accuracy you seek.

June 6, 2023 at 2:04 amWooMin JangSubscriber
I can't fully understand... Just iterate to get the results close to my intial geom??
Well.. the results were almost same as lower figure when i did that

June 6, 2023 at 2:53 pmJim DayAnsys EmployeeSorry to be unclear. What I meant to convey was to remesh your initial geometry so it better represents the unconsolidated geometry (like what it would look like if there were no gravity load). In other words, scale up the geometry so the initial height is around 23.0 so that when it consolidates, the height becomes closer to 20.0. You may have go through some trialanderror to get the right initial geometry. Hope that's clear.

July 23, 2023 at 12:15 pmpeteroznewmanSubscriber
I'm not an expert at LSDyna, but I can share some information about Ansys Static Structrual that is relevant. I'm responding here rather than your new post since this post has the images.
In a nonlinear (large deflection ON) static structural analysis, you can turn on the Inverse Option. That takes an input mesh shape that assumes a load (gravity load in your case) is present at Time=0 and solves for the shape of the mesh that would exist when the gravity load is removed at Time=1. To perform inverse solving, simply set the Inverse Option property to Yes in the Advanced category of the Analysis Settings.
Another way to have the shape of the soil surface remain unchanged when a gravity load is applied is to use the INISTATE command. This command applies a stress to every element in the model at Time=0. If you apply the correct values of stress and a gravity load, then the mesh will be in equilibrium and the mesh won't move at the end of the first step at Time=1.

July 24, 2023 at 5:29 pmJim DayAnsys Employee
LSDYNA does not have an Inverse Option. Your issue seems to be you have a precise target geometry after settlement due to gravity but don't know the associated stress state, and further, you don't know the geometry prior to application of gravity. As for the aforementioned associated stress state, *INITIAL_STRESS_SOLID or *INITIAL_STRESS_DEPTH would allow you to impose an initial stress field. Perhaps the latter would provide a state close enough to equilibrium to suit your purpose.

 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.
 Explicit dynamics ERRORS
 explicit dynamics
 turning simulation
 getting zero maximum and minimum stress value in explicit analysis
 How to figure out impact force in Explicit Dynamic Analysis
 How do get Full values instead of just minimum and maximum ?
 Running an explicit dynamics simulation on a composite plate
 Monte Carlo Simulation
 Euler Domain Restricting Simulation
 How to solve Energy error too large

7742

4502

2963

1449

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