July 26, 2023 at 9:25 amwalter.araujoSubscriber
I’m performing a 2D axisymmetric analysis. The simulation is related to a burst disc subjected to a pressure.
After analysis i found some disc penetration on sharp edge zone. The material disc is aluminium (NL - nonlinear) and contact uses normal lagrange formulation.
It seems this is related to characteristic of material. I found that on 2D axisymmetric analysis is not possible to adjust contact stiffness.
Anyone could help to improve my analysis and avoid this penetration? Any idea or suggestion are welcome
July 26, 2023 at 9:54 ampeteroznewmanSubscriber
Put a small blend radius on the sharp corner. Put at least 6 elements on that blend edge. The contact algorithm will perform much better with the sharp corner removed.
July 26, 2023 at 1:15 pmwalter.araujoSubscriber
July 26, 2023 at 2:25 pm
July 26, 2023 at 2:51 pmpeteroznewmanSubscriber
In the Details of the Contact is a row called Normal Stiffness. Change that to Factor and in the next row, put a Normal Stiffness Factor of 10 instead of 1. That will reduce the penetration. In the row below that you can Update Stiffness on each iteration.
July 26, 2023 at 3:01 pm
July 26, 2023 at 4:46 pmpeteroznewmanSubscriber
Okay, what I said above is only for 3D models.
For your 2D Axisymmetric model, try setting Shell Thickness Effect to No.
July 27, 2023 at 2:58 pmwalter.araujoSubscriber
July 27, 2023 at 9:08 amAkshay ManiyarAnsys Employee
In addition to what Peter suggested, can you try changing the detection method to some nodal or to a combine method?
July 27, 2023 at 3:03 pm
July 27, 2023 at 5:15 pmpeteroznewmanSubscriber
I suggest you change the Behavior from Symmetric to Asymmetric. Make sure the Target side of the contact is the flat plate and the Contact side of the contact is the corner blend.
Then you can retry the two Nodal Normal settings. I can never remember which one is which.
July 27, 2023 at 6:58 pmwalter.araujoSubscriber
– Nodal-Normal From Contact –> disc moves away slightly from fixed part and diverge
– Nodal-Normal To Target –> penetration
July 27, 2023 at 9:09 pmpeteroznewmanSubscriber
I see Small Sliding is On. Turn that Off.
Under Analysis Settings is Large Deflection turned On? That must be On.
Also the Frictionless Contact Behavior is set to Normal Lagrange. You can try some other options.
July 28, 2023 at 1:35 pmwalter.araujoSubscriber
Thank you for your patience.
- Large Deflection turned On? - yes, allways for nonlinear analysis.
- Already tried different types of contact. Despite penetration, "Normal Lagrange" is perfoming better!
- small sliding off - it seems to have a better behaviour but i am facing convergence issues... need more time.
July 28, 2023 at 1:58 pmpeteroznewmanSubscriber
A good remediation for convergence issues is to force the solver to take many substeps. That means setting the Initial and Minimum Substeps to have a large number like 100 or 500 etc. Maximum Substeps should be 1000.
Another remediation is to allow the solver to continue iterations for more than 26 before taking a Bisection by adding the Command object with the code
which will allow the iterations to go to 100 (or 500).
July 30, 2023 at 12:29 pm
July 29, 2023 at 10:33 ampeteroznewmanSubscriber
Another possibility is that the Ansys 2D system was broken at the beginning and is not working properly.
This can happen if you create 2D geometry and open that in Mechanical, but forget to set the Property of the Geometry cell in Workbench to 2D. The geometry is imported into Mechanical as 3D. You build up the model, then realize it is not in the 2D mode so you can't set it to be Axisymmetric. You might expect that you can simply go back to the Property setting of the Geometry cell in Workbench and flip it from 3D to 2D.
While this is possible to do, the outcome is not the same as setting the 2D propertry of the Geometry cell BEFORE ever opening the geometry in Mechanical. The only way to fix the problem is to start a new Static Structural and set the Geometry cell to 2D before you open the Model cell. Then you can build the model and see if that improves the outcome.
July 30, 2023 at 12:34 pmwalter.araujoSubscriber
many thanks for you patience...
I had created a new study as your suggestion but i got not successfully results. Same behaviour!
small sliding switch off improve the study, but it is getting difficult to achieve convergence...
July 30, 2023 at 1:04 pmpeteroznewmanSubscriber
What is possibly happening is the structure becomes unstable at that point.
The static solver may not be able to find a stable equilibrium past that point.
You could try solving the model in either Transient Structural or Explicit Dynamics.
It might also be that a 3D disk wants to buckle out of an axisymmetric shape at some point so a 3D model will give different results in a Transient Structural or Explicit Dynamics solver than the 2D model.
July 31, 2023 at 1:18 pmwalter.araujoSubscriberHello Peter,An explicit analysis is not practiable for me in 2D. It only uses one core and due to the elements size is a study that takes +/-40 hours.Anyway, I think I have arrived at a balanced analysis.It is true that from a certain point the disk jumps out of the rim, and it makes sense that the study diverges (for an implicit analysis).But even diverging I can make an analysis at the moment that the disk jumps, which was actually what I wanted.Conclusion:-small sliding off issue helped me to check the pressure from which the disk release happens (no penetration, even for sharp edge).-use of the transient study allows to "refine" the moment of the disk jump.-In the small sliding there is another option "adaptive", which I think helped too!Peter, thank you very much for your tips and help.
- 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
- User manual
- An Unknown error occurred during solution. Check the Solver Output…..
- 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.
- whether have the difference between using contact and target bodies
- Defining rigid body and contact
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.