April 19, 2018 at 7:52 amMadzRedpathSubscriberI am trying to model a hip with soft tissue impacting the ground using ANSYS 18 Explicit. From a paper, the soft tissue should be modelled as hyperelastic and it used the Mooney-Rivlin model. The values it states are:
C10 = 85.5kPa
C01 = 21.38kPa
I then calcuated d1 to be 9.39e-8.
But when the soft tissue impacts the floor it expands rapidly and the femur just continues to travel through the tissue!
Any ideas why this is happening or how I can fix it?
April 19, 2018 at 11:49 ampeteroznewmanSubscriber
Do you mean the soft tissue is the body mass around the hip, from the skin inward?
What is the impact velocity? What other BCs have been applied?
The Body Interactions item should be sufficient to keep elements from penetrating, but you can also add contact to help the interface from penetrating.
If you attach a Workbench Project Archive file (.wbpz) to your reply, I will take a look at your model. The archive file has to be < 120 MB to attach. If it is larger, you can Clear Generated Data on the mesh, save and the archive will be smaller.
April 20, 2018 at 10:03 amMadzRedpathSubscriber
April 20, 2018 at 1:49 pmpeteroznewmanSubscriber
I am solving your model on 18.2. What version are you using?
I didn't understand why different bodies had different initial velocities, so I set them all to 3.8 m/s.
I also turned off element erosion and turned up the output to 2000 frames. I will check back when it has finished.
April 20, 2018 at 3:05 pmMadzRedpathSubscriber
I am using version 18.1.
Thank you so much for looking at this for me, any advice would be greatly appreciated.
April 20, 2018 at 4:31 pmpeteroznewmanSubscriber
I stopped the above simulation after the first 10 milliseconds to review the results so far.
A few other observations.
1) You have a gap between the floor and the soft tissue. That is just wasting solve time moving them into contact. Make the floor tangent with the soft tissue. I can't change that because I don't have the geometry.
2) I expect the soft tissue to be bonded to the thigh bone and pelvic bone, not left with frictionless contact. I think the soft tissue is just sliding down the bone. I have added bonded contact.
3) I would change the Body Interaction to frictional, since the soft tissue sees friction with the floor.
4) I changed the Mesh size from Default to 10 mm and it made a much nicer mesh and didn't change the solution time much.
5) When you cut the thigh soft tissue, you are removing the support the missing tissue provided. Maybe better to keep the whole thigh. I can change that because I don't have the geometry.
I will rerun these combined with the common velocity changes mentioned above and see what I get.
April 20, 2018 at 8:28 pmpeteroznewmanSubscriber
After you look at that video, you can see that the point mass on the left side of the screen is having an excessive influence on the model. It needs its own spring to impact the floor since it "keeps going" past where it should have been supported by a floor that isn't there.
May 1, 2018 at 10:08 amMadzRedpathSubscriber
I want to thank you so much! You save my final year project and I would love to put you in my acknowledgments section of my report. Are you associated to a university or company?
Thank you so much again!
May 1, 2018 at 10:22 ampeteroznewmanSubscriber
I'm glad to hear your project was a success! Thanks for thinking of putting me in the acknowledgements. You can list me as:
Peter Newman, ANSYS Student Community Moderator
I am not associated with a university. I design products for a medical device manufacturer of digital imaging equipment. I love to learn how to simulate different types of problems, which is why I enjoy helping out here, but I do that in my own time.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.
- explicit dynamics
- Explicit dynamics ERRORS
- turning simulation
- getting zero maximum and minimum stress value in explicit analysis
- Monte Carlo Simulation
- How do get Full values instead of just minimum and maximum ?
- Running an explicit dynamics simulation on a composite plate
- How to figure out impact force in Explicit Dynamic Analysis
- Euler Domain Restricting Simulation
- LS-Dyna not appearing in ANSYS Workbench
© 2022 Copyright ANSYS, Inc. All rights reserved.