November 9, 2018 at 3:25 amzjuv9021Subscriber
I'm working on trying to get a nonlinear 4 layered tubing to be 1. pressurized, 2. bent, and 3. subsequently advanced through an inner rigid tubing and hit a wall and slide past a fixed support:
I have available to me uniaxial, biaxial, and planar shear stress data for 3 out of the 4 materials (Silicone Rubber, PU80A, PU55D). The PU's fit well with a Rooney Mivlin 2 parameter model:
I, however, do not know how to exactly calculate the Incompressibility Parameter for a 9 parameter model... If anyone knows details on how to obtain based on the data I have it would be great. Not confident on how important it is to have this value, I was only provided the data, not the D1 value...
I've also included keyopt, matid,2,1 to introduce Uniform Reduced Integration to all of the nonlinear materials (excluding PET) (To my understanding, this is applied to SOLID185). As it stands, I'm using Linear ordered elements (perhaps quadtratic would elicit better behavior? Unsure) with 200 divisions of sweeps, 2 elements through thickness of the tubes, and 35 divisions around the perimeter, totaling 59,533 elements.
I also decided to bend it halfway (15 degrees) while increasing the pressure in the first substep, as it appeared that my convergence troubles came in the 2nd load step of 30 degrees near the very end. The thought being that I've increased the number of steps over which this load is applied, although not sure if it matters as it appears it's just starting to buckle or becoming unstable near the end.
I've gotten through the bend, but ran into trouble getting it to hit the wall and sliding past the fixed support:
Are there any thoughts on how to get full convergence? Does missing the incompressibility parameter mean a lot in terms of convergence assistance?
November 9, 2018 at 10:33 amSandeep MedikondaAnsys Employee
Zach, incompressibility is very important and will help with convergence. Please see this article on how it is determined and this one on how to deal with it. If you don't have the tests, I would recommend putting in a small value, say 1e-05.
I would also recommend against using any other formulation for the element type, Mechanical typically does a good job of determining this. Drop the mid-size nodes, i.e., use a linear element. I would also try a case with the Ogden material model, you are only fitting data in the tensile range but when buckling the material is compressing and I wonder if there is any material instability there. Keep an eye out on the max. compressive strains your model is experiencing and see how the material fit looks like in that strain range.
In the analysis settings, use a Direct solver for the Solver type and Unsymmetric for Newton-Raphson Option.
Try inserting the following command snippet:
As a last resort, have you already tried adding some stabilization energy, as previously suggested?
If nothing works, report back with the exact error that you are observing?
November 9, 2018 at 2:12 pmzjuv9021Subscriber
I don't have this data yet, and probably won't have the budget for it until next year, but this would be the next step. From this data, could we get the incompressibility parameters?
Additionally, for the Energy stabilization, what is the method for applying? Does "Activation for first substep: On Nonconvergence" Apply after I perform a restart at a specific substep ONLY? Is there a better option here for more overall stabilization?
November 9, 2018 at 4:34 pmSandeep MedikondaAnsys Employee
Zach, it will definitely help. But many analysts don't have this data so you can start with a small initial guess and see if it helps with convergence.
For the question on Stabilization Energy, yes the options you show look good. You ideally don't want to use Stabilization Energy since it is just a numerical tool and not quite physical. You can always try adding a constant amount of energy by selecting yes for throughout the simulation but I wouldn't recommend it. Additionally, you can also turn on Weak Springs and see if it helps.
If the model converges, keep an eye on how much artificial energy is being added in comparison to the total strain energy.
- You must be logged in to reply to this topic.
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.
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.