January 6, 2023 at 11:25 amPierre DrutSubscriber
I'm trying to simulate a seal going over a small steel protrusion as per picture below. The green cylinder will be inserted inside the rubber seal (in red).
I have represented this assembly using an axisymmetric model as represented below.
The issue I have is to go over the small steel protrusion where the elements of the rubber seal become highly distorted.
The seal material is isotropic elastic linear (for simplification).
I have tried a lot of different set-up without success to go over the small steel protrusion: Different mesh size, contact/target set-up, type of contact, formulation, behaviour, contact stiffness behaviour etc...
I would be grateful if someone could help me? I can even share the Ansys model if this is possible?
Thanks in advance,
January 6, 2023 at 12:24 pmpeteroznewmanSubscriber
Use smaller elements around the two circled areas of the rubber part.
Mesh the rubber part with Linear elements, not Quadratic.
Add a small radius to the edge of the steel part and have frictional contact between the radius and the rubber face in the area circled in red.
Is the flat steel ring bonded to the rubber or is there frictional contact?
Use a Hyperelastic material model such as Neo Hookean, rather than a Linear Elastic material model.
While the above may solve the highly distorted element issue, other problems may arise such as convergence failure in a Static Structural model. This is because after the seal reaches the tip of the steel protrusion, it will have a lot of strain energy and will want to snap past the tip. That is a dynamic event which can’t easily be captured in a Static Structural model. There is no static equilibrium just a tiny bit past the tip of the protrusion. This could be overcome by solving in Transient Structural. There are some tricks that can be played in a Static Structrual model to temporarily switch to an explicit dynamics solver to get past the dynamic event.
The other issue is that you are enforcing axisymmetric response, but if you modeled this in 3D, you might find the rubber cylinder buckles into a non-round shape.
If you want to share your model, use File Archive and put the .wbpz file on a File Sharing site such as Google Drive or OneDrive and paste the link to the file in your reply and say what version of Ansys you are using. Members like me will be able to look at your model, but ANSYS Staff are not permitted to download files, so you can only get their help if you post details in your reply of the error messages.
January 6, 2023 at 3:39 pmPierre DrutSubscriber
Thanks a lot for your advises! I have tried using the Transient Structural modul and it did work a lot better, I managed to pass the tiny bit part with the seal. I will now try in 3D to assess if this is making any difference.
I have tried setting up an hyperelastic model in the past (even on very simple model), and I had a lot of convergence issues.
Shall I expect any big differences in the calculation's results (such as train within the rubber part for example) using Transient Structural or static structural?
Many thanks again
January 11, 2023 at 9:51 amPierre DrutSubscriber
Would you be able to assist on my last questions above?
Many thanks again
January 11, 2023 at 11:39 ampeteroznewmanSubscriber
The differences between the strain achieved in a Transient Structural vs a Static Structural are problem dependent. They could be big or small, but in this case, there is no data from Static Structural because there is no solution past the tip of the bump, so Transient is all you have.
There may be differences in strain when changing from a Linear Elastic material to a Hyperelastic material model. However you need to perform a suite of hyperelastic tests on the material and fit the model constants to the material data to get accurate predictions from the 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.
- How to work with STL file?
- Using Symmetry in DesignModeler and Expanding the Results
- Rotate tool in ANSYS Design Modeler
- drawing a geometry by importing a table of points
- section plane
- material properties
- ANSYS FLUENT – Operation would result in non manifold bodies
- Geometry scaling
- Parameters not imported into Workbench 18.2 from Solidworks/Inventor
- Convert Surface body to solid
© 2023 Copyright ANSYS, Inc. All rights reserved.