July 6, 2020 at 3:28 amdshiSubscriber
I'm a new user, so I was wondering whether I could receive some advice on facilitating nonlinear hyperelastic convergence. I have already checked several other threads and online sources, but they do not seem to be enough to help my model converge entirely (Ansystips and this thread were quite helpful though).
I have tried (1) reduced brick integration, (2) fine, linear, tetrahedron meshing, (3) setting initial/min/max substeps and multiple steps with tabular pressure, (4) turning Large Deflection on, (5) constant stabilization, and (6) using Newton-Raphson residuals to identify problematic areas. However, my model always fails to converge at ~7000 Pa, and the model oddly deforms in the opposite direction of the pressure.
I am using my school's ANSYS Workbench 2019 R2 (with no elements/node limits), and applying a pressure of 13332 Pa on a cyclic-symmetric circular diaphragm to measure the resulting displacement and stress. Currently, my analysis settings are 250 initial, 250 min, 1000 max, with Large Deflection on and constant Stabilization.
Here is google folder link containing the archived project file (Warning ~5.6 GB)
Thank you for the help.
July 6, 2020 at 3:45 ampeteroznewmanSubscriber
Without looking at your model, I can recommend reviewing the advice in this tutorial which I just posted today. I might have a chance to look at your model tomorrow as it is too late tonight.
July 7, 2020 at 2:37 amdshiSubscriber
Thank you for the video! I haven't tried to use surfaces to simplify the problem (I thought cyclic symmetry was good enough) or commands. I'll try to implement some of them in a new model and let you know how it goes. In the meantime, it would also be useful for me and my supervisor to see whether the model I sent in the google files is converge-able if possible.
July 7, 2020 at 2:48 am
July 7, 2020 at 11:55 ampeteroznewmanSubscriber
The solid model shown below is meshed with linear tet elements.
A single linear tet element through the thickness of a thin-walled solid is inadequate to capture the bending stiffness accurately.
By contrast, the mesh for the axisymmetric model I provided above has eight linear elements across the thickness.
It would be possible to rotate the faces of these elements into solid elements to create a 3D model from the 2D mesh, but as you can imagine, that will slow down the solution speed by a lot and not necessarily give any benefits. Keep in mind that an axisymmetric solution is a full 3D solution. For example, below is a plot of the hoop stress in the material.
July 7, 2020 at 11:27 pmdshiSubscriber
I see, it does seem like a much more computational-conservative approach to my problem. I initially thought about setting the 3D model's thickness to 4+ elements, but it would have greatly increase the computational power needed.
However, the axisymmetric model is somewhat running into the same problem as my previous model. I was able to reach ~3800 Pa convergence by having three time steps (3000, 5000, 13332 Pa), increasing the substeps, and using even finer element meshing, however I have not been able to progress further. In comparison, the 3D cyclic model is more crude, although it does allow me to reach up to ~7000 Pa convergence.
Do you know whether there any other mesh or analysis settings I can tinker with to help the axisymmetric model converge at higher pressures?
July 8, 2020 at 12:19 ampeteroznewmanSubscriber
One reason that the solid model reaches higher levels of pressure before a convergence issue is because the single element makes the structure stiffer. If you thicken the wall in the outer rings of the structure to add stiffness where the most bending occurs, the axisymmetric model will take higher levels of pressure without a convergence issue. Conversely, if you increase the number of elements through the thickness (or even just use quadratic elements) the solid mesh will be less stiff and I expect it will have convergence issues at lower levels of pressure.
One approach to overcome these convergence issues is to move the problem to an Explicit Dynamics solver. That has no problem with convergence. Maybe I will try that just for fun. The down side is the problem takes a lot longer to solve.
July 8, 2020 at 2:29 ampeteroznewmanSubscriber
Convergence is not a problem in Explicit Dynamics. This is the pressure ramping up to your target value in 1 second. After only .025 seconds, it has reached this position when the pressure is only 333 Pa. The difference is that this is a Dynamics solution, so the momentum in the mass of the part is also a force in the solution which is different to the static solution. The membrane has almost no stiffness to vertical motion initially, so the solution quickly builds up kinetic energy and that is the dominant energy in the system before the internal energy in the stretching of the material begins to develop. A different profile of ramping on the pressure would result in a different amount of deflection at the same 333 Pa of pressure, say if the pressure was rising exponentially instead of linearly, due to the reduction in the amount of kinetic energy at that time.
The solution goes further than this, but at some point, the part deforms to the point where adjacent folds touch and I did not turn on contact to prevent penetration. That is easily done.
Below is a snapshot of a solution that ramps the pressure on much more slowly and the pressure is only 0.0052 Pa. This solution includes the body interaction so that the folds are pressing on each other and not passing through each other. This gives some insight that the solution above has more error than expected because the structure would have passed through this state without contact.
July 8, 2020 at 3:07 pmdshiSubscriber
I was completely unaware that static structural did not take into account deformation due to both kinetic and momentum driving forces. It will be useful for me to verify several of my past designs as dynamic models to more accurately capture what is happening, since some of them under 13332 Pa deformed to about the same extent as the dynamic model at 333 Pa.
Thank you very much for your help and guidance!
- 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?
- 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
© 2022 Copyright ANSYS, Inc. All rights reserved.