October 13, 2023 at 2:17 amMario MongiardiniSubscriber
I am trying to impose a rotation of the deformable part around an arbitrary axis for prepositioning before an impact.
I know that this can be done using *BOUNDARY_PRESCRIBED_MOTION_RIGID_ID if I switch the part to rigid and then manually force its CG to be at the desired centre of rotation by using *PART_INERTIA. However, I need the part to stay deformable for the simulating an impact after the initial prepositioning.
My potential workaround is to create a *CONSTRAINED_NODAL_RIGID_BODY_INERTIA using the nodes of the deformable part that I want to rotate so that I can leave the original underlying part deformable and impose the an arbitrary CG location of the overlaid CNRB. Based on the LS-DYNA manual, a rotation imposed to this CNRB through *BOUNDARY_PRESCRIBED_MOTION_RIGID_ID will occur around the CG defined through the manual inertia assignment to the CNRB.
However, the rotation imposed to this CNRB still occurs around the original CG of the CNRB and not the node used to manually impose its new inertia properties.
Is this due because LS-DYNA gives priority to the inertial properties of the underlying deformable parts? Or is it a bug in the code?
Any suggestion to make it work would be helpful.
October 13, 2023 at 3:58 pmJim DayAnsys EmployeeIf you just want to reposition the deformable body before the analysis, the more straightforward approach would be to do that using a preprocessor (LS-PrePost or other) and save a new keyword input file with the system in the desired configuration. I'm assuming you want to start the simulation with parts in an unstressed state.
October 15, 2023 at 5:21 amMario MongiardiniSubscriber
I was already aware of the option you are suggesting, but unfortunately that will not work well in my case as I need to re-start the simulation including the prepositioning stress.
The additional option to carry over alos the initial stress from the dynain file does not appear to work well either as the model includes some parts that make use of MAT_FABRIC, for which stress cannot be carried over using the dynain file.
October 16, 2023 at 2:47 pmJim DayAnsys EmployeeI want to understand the situation. Are you saying the pre-positioned parts are prescribed some initial stress via *INITIAL_STRESS_... and those stresses must only be transformed due to the repositioning? Or are there additional stresses/deformation imposed due to the repositioning, e.g., from contact with other parts, inertial effects, etc?
October 17, 2023 at 8:49 amMario MongiardiniSubscriber
The latter case – the imposed rotation of the rigidised part (skull of GHBMC) is causing to the neck of the human body model to deform with comsequent stress and strains of those pasrt to be carried over in the secodn simulation.
I can definitively carry over the deformed configuration using either the dynain or exporting the nodes at any desired state from LSSP, but I cannot apply intial stress to some parts that make use of MAT_FABRIC during the second run.
My goal is to use a simple restart to run a drop test after having preposited the head (with the corresponding deformed neck). However, I also need to turn the rigidised skull (with manually assigned inertia properties for the prescribed centre of rotation) back to deformable. And this appears to be possible only if I use a CNRB, which can be turned off the end of the propsotioning simualtion.
October 17, 2023 at 2:33 pmJim DayAnsys EmployeeMaybe I'm not thinking clearly yet this morning, but could you make use of *DEFORMABLE_TO_RIGID_AUTOMATIC on the skull to toggle between rigid and deformable? Or is that approach somehow not compatible with the positioning you need to do? If you're a commercial customer, you can file a case and provide a simple test case to illustrate your dilemma. Unfortunately, the forum does not allow sharing of files.
October 20, 2023 at 1:28 amMario MongiardiniSubscriber
Unfortunately, when I toggle the deformable skull to rigid using *DEFORMABLE_TO_RIGID_INERTIA, then LS-DYNA appears to still consider that part as deformable in the *BOUNDARY_PRESCRIBED_MOTION_RIGID and therefore I get an error message that the part assigned is not rigid.
My intial idea of defining a CNRB is compatible with using *BOUNDARY_PRESCRIBED_MOTION_RIGID, but unofrtunatley LS-DYNA appears to neglect the imposed CG using the intertia feature despite the manual says if should use what imposed manually. Maybe something to consider in the next debugging of the LS-DYNA code by Ansys?
October 20, 2023 at 1:44 pmJim DayAnsys EmployeeWhat version of LS-DYNA are you currently running (R13.1.1, R14.0.0, ?). Look in the banner of your d3hsp file.
October 24, 2023 at 12:32 amMario MongiardiniSubscriber
I am using LS-DYNA Revision: R13.1-138-g8429c8a10f
I will try using the latest release of LS-DYNA to check if this can solve this issue.
October 24, 2023 at 2:37 pmJim DayAnsys EmployeeConfirmed that even using version dev, *BOUNDARY_PRESCRIBED_MOTION_RIGID cannot be used on a part that has been switched from deformable to rigid using *DEFORMABLE_TO_RIGID_INERTIA.
October 24, 2023 at 5:32 pmJim DayAnsys EmployeeTry this. Leave the skull deformable, define a node set containing the skull nodes, and use *BOUNDARY_PRESCRIBED_MOTION_SET to rotate those nodes about an axis that is parallel to either the x, y, or z global axis. Do this by setting DOF=9,10, or 11. OFFSET1 and OFFSET2 locate the axis of rotation. You can specify a death time (DEATH) to release the node set from the prescribed motion.
- 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.
- 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.