Tagged: convergence, load-step, loadstep, static-structural, timestep
February 1, 2022 at 3:52 pmInes_Subscriber
I am performing an Static Analysis that consists on putting a pressure of 10 Pa on a model with hyperelastic materials and contact.
After strugging with convergence problems, I found out that there is an unstable position in my simulation because each time I run it crashes at the same point (5Pa). To give you an idea, the model of my simulation goes from one stable position to another stable position.
I took control of contact (pinball, formulation) and set Unsymmetric Newton-Raphson method and it was better but I still had convergence problems.
Then, I tried decreasing time step... and it didn't help. However, what worked was putting 5Pa on a Load Step and 5Pa more in the next Load Step. And I don't understand why.
I took care of having equivalent Time Stepping for both analysis. For example, in the 10Pa per LoadStep case I set initial step number to 10 and in the 5Pa+5Pa case I set initial step number to 5 in each Load Step: in both analysis the initial preassure was 1Pa. I did the same with the max and the min step number.
This makes me think that is not the same applying a pressure in one Load Step than applying half and half in two Load Steps in an Static Analysis and I don't understand why. Is there any logical reason for this behaviour? Does Ansys do sth different when going from one Load Step to another that doesn't do when passing from one substep from another?
Thank you very much,
InésFebruary 2, 2022 at 3:15 ampeteroznewmanSubscriberDear In├®s You can try Transient Structural and let dynamics help your structure go through the unstable state.
February 2, 2022 at 9:38 amInes_SubscriberDear Peter,
thank you for your advice!
But I am still curious about why applying the same load in one or two Load Steps in an Static Structural Analysis is not the same.
February 2, 2022 at 11:02 amRameez_ul_HaqSubscriber,in order to understand that, please go through the playlist provided by ANSYS on ANSYS Learning YouTube channel, which goes as:
'Computational Resources Considerations - Ansys Innovation Course'
'Large Deformation - Ansys Innovation Course'
'Structural Nonlinearity - Ansys Innovation Course'
February 2, 2022 at 5:13 pmpeteroznewmanSubscriberDear In├®s In a nonlinear solution involving hyperelastic materials, the best strategy is to force the solver to take many small steps. This is accomplished by setting the Minimum Substeps to a high number.
In Static Structural, under Analysis Settings, turn on Stabilization which can help structures get past an unstable deformation.
February 3, 2022 at 9:09 amInes_Subscriber
Thanks for the advice!
Increasing min substeps is the strategy I followed but, is it possible that some problems don't converge even with a great number of substeps? Because that was the feeling I had in my simulation.
February 3, 2022 at 12:14 pmpeteroznewmanSubscriberDear In├®s There are many reasons why a solution will fail to reach the end time. Sometimes an error occurs, such as the "highly distorted element" error. This is resolved with better element shapes. Let's exclude that from the question you ask.
There are Static Structural models where the solver fails to find equilibrium when increasing the load by a small increment. A common scenario is in structures that have a snap-through behavior. The normal load incrementing method fails, which is what you were experiencing. If the load could get past the instability, there is a statically stable configuration on the other side of the instability, but the normal algorithm can't get there. That is what turning on stabilization does, it introduces artificial forces to stabilize the structure to get it past the instability to get to the other side.
There are other technologies that can be helpful with hyperelastic materials that reduce the difficulty the solver has in finding equilibrium. One of those is called the mixed u-P element formulation. Without that, the deformation of the nodes determines the pressure in the element. That is normally fine because the material is compressible and small changes in nodal deformation creates small changes in element pressure. But hyperelastic material can be incompressible or nearly so with Poisson's ratios of 0.49 or higher. Now small changes in nodal deformation creates huge changes in element pressure, which makes find equilibrium very difficult. The mixed u-P element formulation adds a pressure degree of freedom to the element making it much easier to find a set of nodal deformations that have equilibrium. You should definitely be using this in your model.
Best regards Peter
February 4, 2022 at 9:37 amInes_Subscriber
Thanks for such an amazing answer!! I wasn't aware of this tips. Thank you for the detailed explanation!
Viewing 7 reply threads
Ansys Innovation Space
- 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.Trending discussions
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- 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
- 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.
- Colors and Mesh Display
- User manual
- material damping and modal analysis
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.