November 28, 2019 at 9:44 pmsamuelchristSubscriber
Dear Ansys Community,
I am trying to simulate contact between Polyurethane Disk and the inside of a Steel Pipe in order to measure the frictional force experienced by the disk. The model that I use is Axisymmetric 2D. The problem that I constantly face is that the disk penetrates the thickness of the steel pipe even though the contact between the two is defined as Frictional with a friction coefficient of 0.4
Any suggestions to solve this problem? The link below is the Ansys project file.
December 2, 2019 at 9:25 amAniketAnsys Employee
ANSYS employees are not allowed to download files from the student community, so hopefully, others can help in this regard.
If you want to reach a broader audience, kindly insert the images inline in your post instead of external links.
Generally, the Friction coefficient does not affect penetration. It will affect the force that is required for sliding the two parts together.
How much is the penetration? If the contact is detected and you want to reduce the penetration in the contact you will need to increase FKN i.e. Normal stiffness of the frictional contact.
Guidelines on the Student Community
December 2, 2019 at 2:22 pmpeteroznewmanSubscriber
I opened your axisymmetric (Y axis) model.
The problem in your model is that you have assigned an X=0 displacement to the entire top edge of the pig.
The pig cannot compress except on the radius with that boundary condition.
I suggest you make the following changes to the model.
- Delete the Fixed Support and the Displacement BCs.
- Add a Frictionless Support to the top edge of the pig.
- Add a displacement BC to the outer edge of the pipe, X = 0 and Y = 5 mm
- Turn on Auto Time Stepping
- Set the Initial Substeps and Minimum Substeps to 100
- Add a Command to Static Structural to make it keep iterating for longer than 26. NEQIT,100
- Increase the Mesh to Resolution 3
- Change the Contact Normal Stiffness back to its default value of 1
Now the pipe will move up and the pig is free to be compressed but that is not enough. The convergence stops after 1.25 mm.
One way to help it converge is to draw a more gradual compression profile on the pipe entrance. Another way is to add a remote displacement to the end of the pig to compress it, then move the pipe up then deactivate the remote displacement. I have done a part of this below, but I haven't put it all together.
I expected a pig to be a much longer object, but perhaps this is just the scrapper and there is a much longer carrier that keeps it aligned in the pipe.
- 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
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- 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
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.