October 9, 2018 at 7:58 pmzjuv9021Subscriber
I'm trying to model a tubing that is essentially compressed, hits a wall above it at varying heights, slides towards the fixed and potentially occludes, this can be seen in the crude drawing below:
Please see attached .wbpz archive. Seems fairly straightforward, but am getting my elements blown up and abrupt changes in contact as soon as the tube hits the above wall. I set my pinball to be fairly large and have it predict for impact with still no success.
Any thoughts or solves would be greatly appreciate so I can understand the failure of mechanisms here.
October 10, 2018 at 12:42 ampeteroznewmanSubscriber
You want to reduce your model to the minimum that is required to get some useful information. You have geometry for the handle that is attached to the tube, and you are holding that handle fixed.
Suppress the Handle body and move the Fixed Support to the end of the tube that was fixed to the handle.
The tube is pushing against a flat wall solid body that is much, much stiffer than the tube. Change the flat wall from Flexible to Rigid and the solver doesn't have to calculate the practically zero deformation in the wall.
The next change you need is to put at least 4 elements through the tube wall thickness. You have two or three.
I made the length of the elements a bit longer than I wanted, but this was just to get a first result. See that the rigid surface only has surface elements.
That mesh was able to solve to 60% of the full load before failing.
This took only 111 seconds to solve on 8 cores.
Here is the deformation at 60% load. I didn't check how far you got with your initial model.
I got the same error message you did.
Here are the elements that are failing. They are at the Remote Displacement end.
The corrective action to get the model to make more progress to the full load is to use smaller elements near the end.
There may be an advantage to change the Behavior of the Remote Displacement from Deformable to Rigid, but maybe not. Have to run it both ways to see which one goes further. With those two changes, it got to 76% of the load.
The problem now is just force equilibrium convergence. This solution took 1009 seconds on 8 cores.
There are no more element errors. The next step might be to switch from Static Structural to a dynamics solver since finding equilibruim states from this point forward is going to be very difficult. What speed it the end moving?
Another change that might help down the road is to change from a linear elastic isotropic material to a hyperelastic material.
October 10, 2018 at 3:56 amzjuv9021Subscriber
Thank you very much, Peter.
Ultimately, the end goal is to view the mechanism of failure after this tubing is displaced as is seen in my crude drawing above, the speed at which this happens is not important. We have witnessed in real world application that if this happens, then the tubing is highly susceptible to occluding, I'm wondering how I can get to this point to demonstrate?
Having said that, would a dynamic solver still be beneficial in finding equilibrium? Otherwise, would switching over to hyperelastic perhaps assist in equilibrium as well?
October 10, 2018 at 11:42 ampeteroznewmanSubscriber
The solver stopped with Element Violations.
Stay with Static Structural until convergence problems cannot be overcome.
Right now change material model to hyperelastic. There are some posts here to research which hyperelastic model to use as there is a long list to choose from.
Here is a post with some "tricks" to help elements support the large strains that will be developed in this model.
- 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.