July 2, 2021 at 3:18 pmayush_3Subscriber
I am modelling a hyperelastic model for which I have the uniaxial tension and shear data. I did curve fitting with the Ogden 1st order material model, but it shows the following error when I ran the analysis:July 3, 2021 at 10:03 pmpeteroznewmanSubscriberDon't leave the Incompressibility Parameter as 0. Calculate a value and use that. See this discussion.
July 4, 2021 at 4:08 amJuly 4, 2021 at 12:32 pmpeteroznewmanSubscriberIn Engineering Data, create a new material. Add Ogden 1st Order. Type in the three constants. In Mechanical, assign this new material to the solid body in the Geometry branch. Does it start working?
July 4, 2021 at 1:47 pmayush_3SubscriberNo sir, it didn't work. I have seen a lot of Youtube videos; they all do the same thing. There have to be some differences arising due to the version I am using, Ansys 2021 R1. There was a similar error due to the version settings, see my previous post on the Ansys forum here:
I can't get to such errors all by myself, and I need your help.
July 4, 2021 at 4:48 pmpeteroznewmanSubscriberI opened one of my hyperelastic models using ANSYS 2021 R1 and did the steps described above and it worked for me. There much be something else wrong with your model. Please use File Archive to create a .wbpz archive and attach it to your reply. I will take a look.
July 4, 2021 at 5:26 pmayush_3SubscriberThat's so great of you sir, please see the file attached below.
July 4, 2021 at 6:36 pmpeteroznewmanSubscriberI immediately see why you get an invalid property error. You are using a Modal analysis. Modal analysis is a Linear analysis. No nonlinear properties are allowed in a Linear analysis. If you use a Static Structural analysis, you will see that this nonlinear material works fine.
I noticed that your mesh is inadequate. It has only one solid element through the thickness. You should add Mesh controls to ensure at least 4 elements through the thickness. It is sometimes better to use Linear elements rather than Quadratic elements for Hyperelastic materials.
July 4, 2021 at 7:07 pmayush_3SubscriberSir, then is there no way to analyze the vibrational analysis with hyperelastic material properties? I have to apply the Triangular shocks, which were, I suppose, only possible through Random Vibrations for which Modal is a pre-requisite. And my project guide wants me to use the hyperelastic material.
July 4, 2021 at 8:05 pmpeteroznewmanSubscriberPlease describe in detail the analysis you need to do. Describe in detail the "Triangular shocks" load.
It is possible to apply a series of triangular profiles of acceleration vs time in a full Transient Structural model and obtain the transient response of the structure and use any nonlinear behavior you want such as contact, large deflection and hyperelastic material. No Modal analysis is required.
If you have a linear system, you can use a Modal analysis and feed the modal results into the setup cell of a Transient Structural model to get a transient response in much less time than the full Transient Structural with no Modal.
A train of triangular shocks is not a random vibration.
July 5, 2021 at 4:02 amJuly 5, 2021 at 4:18 ampeteroznewmanSubscriberOkay. You can do that with a Transient Structural analysis. Just convert the g load to m/s^2 by multiplying by 9.8 and you can apply that load when the units are set to SI units.
Make sure to include some damping in the simulation.
Viewing 11 reply threads
Ansys Innovation Space
- 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.Trending discussions
- How to calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
Top Rated Tags
© 2022 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.