February 15, 2022 at 9:16 pmchuber3Subscriber
I ran the same head model simulation locally on a SMP double precision solver and on a high performance computing system using an MPP double precision solver. The model uses an acceleration input at the head center of gravity to drive the model. The acceleration at many nodes were similar; however, the strain values were substantially different throughout. Not sure what is causing these strain values to be significantly different for the same input .k file.February 16, 2022 at 9:51 pmReno GenestAnsys Employee
How different are the strain values? It is possible to get small differences because the SMP and MPP implementations are different. This is especially true for contacts. Do you have contacts in the model? Have you reviewed the contacts in the results? If one or multiple contacts are not detected properly with one solver and it works with the other, then you might get strain results that are significantly different.
Are you able to reproduce the problem on a simple cube or even a single element model with no contacts? If so, then there might be issues with the material model.
Let me know how it goes.
February 18, 2022 at 4:24 pmchuber3SubscriberThank you Reno,
The strain values are 0.04 compared to 0.12; however, the time series and shape are completely different. It does appear that contacts are causing the issue. There are 5 contacts, and we believe that the contact causing the issue is *CONTACT_SLIDING_ONLY_PENALTY for the contact between the brain and surrounding CSF.
Is there an equivalent contact that can be used for MPP or can the contact be configured to MPP?
February 18, 2022 at 5:40 pmReno GenestAnsys Employee
Unfortunately there is no "SMP to MPP" switch for contacts. Make sure the contact works in MPP. Compare the penetration for this specific contact in SMP and MPP. Try to have the same behavior in MPP. If too much penetration in MPP, you can change the SOFT=0,1,2. Also, you can try SOFT=2, SBOPT=3 or 5, and DEPTH=33 or 35.
I am not so familiar with *CONTACT_SLIDING_ONLY_PENALTY and I wonder if it is the right contact for your brain application. Here is what the user manual says about sliding contacts:
"Sliding only contact is one of the oldest types. There are two versions
SLIDING_ONLY and SLIDING_ONLY_PENALTY. The first is constraintbased
while the second is penalty-based. Sliding only contact restricts the
nodes of SURFA to slide along SURFB. No separation is allowed with
these methods. These contact types are useful for treating interfaces
where the gaseous detonation products of a high explosive act on a solid
material. See the theory manual for more details."
Also, this presentation says that sliding contacts are for high explosive gas to structure interactions:
And the LS-DYNA theory manual says the following:
"29.11 Sliding-Only Interfaces
This option is seldom useful in structural calculations. Its chief usefulness is for treating
interfaces where the gaseous detonation products of a high explosive act on a solid
material. The present algorithm, though simple, has performed satisfactorily on a
number of problems of this latter type."
How is the CSF modeled? Is it an ALE fluid? Or is it simplified and modeled as a Lagrangian solid?
February 23, 2022 at 8:13 pmchuber3SubscriberThe CSF is modeled as an ALE Fluid. The other surface contacts in the model between CSF and brain components were set up as tied surface-to-surface offsets. Therefore, we changed the contact from a sliding penalty to match the surface-to-surface offsets of the other contacts, and this appears to have fixed any issues. Now, the results are quite similar from SMP run locally and MPP run on a high performance cluster. I am consulting with the original creators of the model to confirm validation.
Thank you so much for the help and information!
Viewing 4 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.