November 27, 2018 at 10:46 amF. Semih YSubscriber
I try to simulate pressure on a hyperelastic material (TPE) in contact with an object. I fitted only uniaxial test data (not compressive nor shear) and used the 9 parameter moonley-rivlin model.
Are there any setting recommendations to obtain convergence? At contact moment the simulation fails. Solver settings are all on program controlled except for large deflections of course. I tried all different contact relations.
Currently i get the following warning:
The solver engine was unable to converge on a solution for the nonlinear problem as constrained. Please see the Troubleshooting section of the Help System for more information.
November 27, 2018 at 11:24 amjj77Subscriber
It could be the contact or the material (since you do not have large deflections on).
Try these out. In order to try if it is the material use linear elastic properties (just some steel properties). If that works then it is the properties (graph and test data look strange in my view).
If this does not work then it is the contact (or something related). From the image above it is hard to see what is going on. Anyway make sure that the restraints are OK.
Hope this helps. If not feel free to attach/provide the model (assume there is no secrecy, should not be since this is a student forum) somehow here so someone can have a look.
November 27, 2018 at 3:20 pmpeteroznewmanSubscriber
I recommend a few things in addition to turning On Large Deflection, which you have already done.
1) Turn On Stabilization under Analysis Settings.
2) On the Contact between the object and the hyperelastic sheet, under Advanced, change the Normal Stiffness Factor to 0.1
3) Break the load into multiple steps. The first step should take the panel to just before touching the object, then second step can have a large number of Initial and Minimum Substeps to help the solver gradually make contact with the object.
November 27, 2018 at 4:52 pmF. Semih YSubscriber
With a linear elastic material i have no problems for friction values above 0.2. (Large deflections is on, with large deflections off the result is extreme and contact is ignored) But i do get warnings:
One or more contact pairs are detected with a friction value greater than 0.2. If convergence problems arise, switching to an unsymmetric Newton Raphson option may aid in convergence.
Contact status has experienced an abrupt change. Check results carefully for possible contact separation.
result (contact pressure):
If I use the exact same conditions but change the material to hyperelastic, i get the following warning:
Element 214 located in Body "test contact plate cilinder-prt1Solid1" (and maybe other elements) has become highly distorted. You may select the offending object and/or geometry via RMB on this warning in the Messages window. Excessive distortion of elements is usually a symptom indicating the need for corrective action elsewhere. Try incrementing the load more slowly (increase the number of substeps or decrease the time step size). You may need to improve your mesh to obtain elements with better aspect ratios. Also consider the behavior of materials, contact pairs, and/or constraint equations. If this message appears in the first iteration of first substep, be sure to perform element shape checking. Named Selections for the offending element can be created via the Identify Element Violations property on the Solution Information Object.
result (unconverged) after 5e-2 seconds.
When increasing increments with following analysis settings:
I get the same error, 'highly distorted'
When I suppress the contact, the simulation (with default analysis settings) runs fine up until some maximum strain (25%). I solved this by using a step (1 second) applying a load until 25% strain, and the next step (1 second) to get from 25 to 25.7 %.
I looked at my hyperelastic data to see what behaviour the material shows at this critical strain of approximately 25% . I see that there is a curve starting around that strain percentage. Could this be the reason? Does it also mean that the increment can be larger again after 50% because the line is quite linear? Can the program take this into account with some settings or do I have to refine the analysis settings manually? Also, I do not expect to have a strain larger then say 300%. Do I save simulation time if I reduce my data? Because judging by the curve, I can fit a 2nd order polynomial instead of a 3rd order up until 350%.
November 27, 2018 at 6:09 pmpeteroznewmanSubscriber
I recommend you use a much finer mesh on both the hyperelastic panel and the object around the contact region. I think the reason for the non-convergence is that the mesh is too coarse.
What kind of elements is the panel meshed with?
You might try shell elements if you currently have solid elements.
If you have solid elements, you should have at least 3 elements through the thickness.
You can also try SOLSHELL190 solid elements as they are made for thin structures.
Other members may have other ideas.
November 28, 2018 at 9:17 amF. Semih YSubscriber
Currently experimenting with all suggestions. My mesh settings are also all default (Adaptive) And I indeed have a thin structure. Meanwhile an answer for the questions regarding the material data fitting?
I looked at my hyperelastic data to see what behaviour the material shows at this critical strain of approximately 25% . I see that there is a curve starting around that strain percentage. Could this be the reason? Does it also mean that the increment can be larger again after 50% because the line is quite linear? Can the program take this into account with some settings or do I have to refine the analysis settings manually? Also, I do not expect to have a strain larger then say 300%. Do I save simulation time if I reduce my data? Because judging by the curve, I can fit a 2nd order polynomial instead of a 3rd order up to 350%
see graph last post
November 28, 2018 at 9:25 amAshish KhemkaAnsys Employee
Can you check the incompressibility parameter in your model? A zero value for this parameter also causes convergence issues. You may use a small value of incompressibility parameter - (say 1e-6) because the material cannot be fully incompressible.
April 5, 2020 at 8:51 pmyy4g17Subscriber
Hi, I am currently trying to simulate the same problem, with a inflated tyre contacting ground, I think the problem described in this thread also applies to me. How do I change the element type from the default (SOLID186-187) to something else such as hyperelastic element?
April 6, 2020 at 1:19 ampeteroznewmanSubscriber
Hyperelastic is a material model. You create a material in Engineering Data and choose a model from the Hyperelastic category. You don't need to change the element type. You might need some keyops to make the element work better with incompressible materials.
April 6, 2020 at 2:22 amyy4g17Subscriber
Yes, changing the keyops was what I meant, are you familiar with the relevant APDL commands to modify the keyops? Or are there existing tutorials online? I've tried the mechanical APDL itself, but it is not very new user friendly...
April 6, 2020 at 11:04 ampeteroznewmanSubscriber
This post uses an older version of Workbench, so the user interface is a bit different now, but it shows how to apply keyops to elements on bodies.
- 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.
- How to calculate the residual stress on a coating by Vickers indentation?
- Solver Pivot Warning in Beam Element Model
- Errors – Reinforced Concrete Beam
- An Unknown error occurred during solution. Check the Solver Output…..
- 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
- Massive amount of memory (RAM) required for solve
- Cannot apply load on node
- Colors and Mesh Display
- Large deflection