February 14, 2022 at 4:48 pmMohammadMahdiSubscriber
I recently moved from SMP-single precision to HPC-DMP-Intel MPI to reduce runtimes. However, there is a contact loss now between the rigid finite elements hitting target finite elements. This issue did not exist when I used to implement SMP. FYI, I'm using Eroding_Surface_to_Surface contact card.February 16, 2022 at 9:44 pmReno GenestAnsys Employee
There are differences in the contact implementation for SMP and MPP LS-DYNA and so it is possible to get different results. You will have to change contact settings to get similar results.
February 16, 2022 at 10:04 pmMohammadMahdiSubscriberHi. Thanks for your reply. What do you mean by changing contact settings? What should be changed specifically to get the same results? Thanks.
February 16, 2022 at 10:16 pmReno GenestAnsys Employee
Without the model, it is difficult to say. But, if one part goes through another part, I would try with different SOFT options (0, 1, 2). Also, you can try SOFT=2, SBOPT=3, and DEPTH=33 or 35 and PSTIFF=1. After that, you can play with the contact stiffness.
Also, I recommend you learn about LS-DYNA contacts:
Let me know how it goes.
February 16, 2022 at 10:39 pmMohammadMahdiSubscriberThanks for your suggestions. I changed Eroding_Surface_to_Surface contact to Eroding_Node_to_Surface contact and it worked. Now Rigid finite elements (impactor) hitting target finite elements (composite) can recognize each other successfully. But there is one more issue here. My target is composed of two parts: finite elements and SPH nodes. I use Tied_Node_to_Surface_offset to tie these two materials together but I get this error:
Please let me know if you have any idea. Thanks.
February 16, 2022 at 10:47 pmReno GenestAnsys EmployeeHello @MohammadMahdi
The node is not tied. Try setting SST=-1 and MST=-1. You need to set SST and MST to a negative value larger than the gap between the node and the segment and it should get tied. The value of -1 may be a bit too large, but it should work.
Let me know how it goes.
February 17, 2022 at 2:02 amMohammadMahdiSubscriberHi Reno. Thanks, it worked. Setting SST and SMT to -1 removed the contact warning and tied successfully the SPH nodes to the adjacent finite elements.
In order to remove artificial waves coming from boundaries in impact modeling, non-reflecting boundary condition (NRBC) is suggested. However, as I've seen so far in my models, NRBC does not work well for SPH nodes except for the fixed SPH nodes. I mean, non-fixed SPH nodes are deactivated when NRBC is applied. Do you have any idea in this regard? Is there anything else playing the same role as NRBC for non-fixed SPH nodes? FYI, I usually fix the bottom SPH nodes, and the side SPH nodes making my target are free. Thanks in advance for sharing your thoughts.
February 17, 2022 at 4:02 pmReno GenestAnsys EmployeeHello @MohammadMahdi
I would start a new thread for non-reflecting BCs; it is different than contact loss with MPP.
February 24, 2022 at 2:50 amMohammadMahdiSubscriberHi Reno, I did. Thanks.
Viewing 8 reply threads
Ansys Innovation Space
- You must be logged in to reply to this topic.
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.Trending discussions
- explicit dynamics
- Explicit dynamics ERRORS
- turning simulation
- getting zero maximum and minimum stress value in explicit analysis
- How do get Full values instead of just minimum and maximum ?
- How to figure out impact force in Explicit Dynamic Analysis
- Monte Carlo Simulation
- Running an explicit dynamics simulation on a composite plate
- Which analysis to use for dynamic and quasi-static compression of auxetic structures?
- Euler Domain Restricting Simulation
Top Rated Tags
© 2023 Copyright ANSYS, Inc. All rights reserved.Ansys does not support the usage of unauthorized Ansys software. Please visit www.ansys.com to obtain an official distribution.