May 12, 2023 at 1:26 pmZeinabSubscriber
I am carrying out a hyperelastic simulation with Ecoflex-30 as a material (Yeoh 3rd degree model, with the following characteristics: C1 = 17 kPa, C2 =-0.2kPa , C3 = 2.3e-2 kPa).
As shown in the following photo, I am carrying the simulation on a thick cylinder of internal radius ri = 8 mm and external radius rex = 10 mm. The total length of the cylinder is 58mm. One end of the cylinder is fixed while its interior is pressurized with air.
The simulation is carried out with 100 steps (auto time stepping on. Initial, Minimum, and Maximum substeps all set to 100. Large deflections are activated. I set Keyopt(6) = 1 for the body as I have seen that it helps the solution to converge. The mesh is tetrahedral.
No matter what I do the simulation always fails at the same point (at 58%). I tried increasing the number steps from 100 to 250, refining the mesh, activating/deactivating the nonlinear adaptive region, increasing the number of substeps, etc... but the solution always fails at the same point (58%).
Before, the error stated that SOLID187 is experiencing high distortion but after some modifications the error only says that the solution can't converge at a substep of this step...
Do you have any idea how can I fix this problem?
Thanks in advance.
Note: I have to use a yeoh model for the ecoflex-30
May 13, 2023 at 10:52 amAkshay ManiyarAnsys Employee
Convergence can be very tricky to solve with all kinds of non-linearity. Please check the below Ansys video on handling distortion issues with Hyperelastic material. You can try the changes explained in the video and see if it helps.
Also, try to check the Newton-Raphson residuals and element distortion to check which location is having issues. After finding the problematic region, you can check for the issue and make changes accordingly.
How to access Ansys help links
Guidelines for Posting on Ansys Learning Forum
May 13, 2023 at 4:33 pmpeteroznewmanSubscriber
The key to understanding why this model consistently fails to converge at 58% of the pressure load is to observe the slope of the total deformation plot. Look at the last few converged points. The slope is getting steeper and steeper and is approaching a vertical asymptote.
The solution logic applies increments of pressure and solves for the displacement (deformation) of the nodes that create static equilibrium between the internal stress and the applied load. In this model, looking at the slope of the total defromation plot, you should expect the next increment of pressure will require an infinite total deformation. In other words, the structure is approaching an instability where there is no static equilibrium solution for the next increment of pressure. To resolve this problem, either turn on Stabilization under the Analysis settings or change the analysis to Transient Structural. In a transient solution, the structure is not required to be in static equilibrium at each time step, it can accelerate elements that are out of balance with the applied forces and internal stresses and find dynamic equilibrium at each time step.
An example which is easy to understand is a hyperelastic dome. As the pressure is applied to the convex top side of the dome, it deforms downward, but at some point, it wants to snap through and the top side becomes concave. A Static Structural solution will fail to get the dome to the concave state without turning on Stablization or changing the analysis to Transient Structural.
- 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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.