June 24, 2020 at 6:28 pmN0834237Subscriber
I'm unsure which one to use and they both give very different results, I was told that it doesn't matter however the results should be the same otherwise. Picture will be posted on next post, right or left contact selection?
right picture - only the pure contact surfaces selected when the cylinder compresses onto the lattice face
left picture - the whole body itself selected for the target and contact, (there are only two bodies the lattice and the cylinder no smaller components)
June 24, 2020 at 6:29 pm
June 24, 2020 at 6:39 pmSaiDAnsys Employee
From the two images, the contact on the right side should suffice if the the honeycomb structure does not get crushed. But if it does get crushed, then some of the side faces might come in contact with the cylindrical block, but since contact isn't defined between them, the side surfaces won't detect contact (and hence penetration will occur). So if crushing occurs, then at least the lateral faces of the honeycomb should be included in the contact.
Another thing to note is, when contact occurs between an edge and a surface (like the edges of the honeycomb are coming in contact with the flat surface), the flat surface should be the target side and the geometry with the edges should be the contact side. The reason is that contact detection points are on the contact side and hence they need to be on the edges to minimize penetration.
Another reason I can think of is that the pinball radius may be different for the two cases, so initial contact may be detected between more number of element pairs in the two cases. You can use the Contact Tool to find the Initial Contact Status between the two cases to compare them.
Hope this helps,
June 24, 2020 at 6:52 pmN0834237Subscriber
The honeycomb is crushed in the sense that the height is 37mm, but the compression from the cyclinder is 25mm, so would the left selection be better and swapping the target and contact ofc so that the target is the flat cylinder.
June 26, 2020 at 7:55 pmSaiDAnsys Employee
Yes, in that case the first selection would probably be better. If during the course of crushing different faces of the honeycomb touch each other, you probably also need to assign self-contact for the honeycomb.
Hope this helps,
July 1, 2020 at 10:22 amN0834237Subscriber
Is there an easier way of applying self contact or do I have to define contact for each face on the honeycomb as it self penetrates, also would that change the force displacement results?
July 1, 2020 at 1:49 pmSaiDAnsys Employee
If you know which pairs of the honeycomb faces interact with each other, you can define the contact pairs which would be computationally more efficient. But if that is not clear and you need to define self-contact (i.e. each face can get crushed and bent and hence come in contact with itself), you could just select all the faces, create a Named Selection and used that Named Selection for both Contact and Target sides and define the Behavior to be Symmetric.
For easier Selections, you could select one of the faces of the honeycomb, then go to the Ribbon on top -->Selection tab-->Size--> Select All Entities with the Same Size.
If there is self-contact happening physically, but it hasn't been defined in the simulation, the simulation will probably give a softer response. So in that case, defining the self-contact will give a stiffer force-displacement response.
July 1, 2020 at 3:18 pmN0834237Subscriber
Thank you for your 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.
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- 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
- whether have the difference between using contact and target bodies
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Colors and Mesh Display
- material damping and modal analysis
© 2023 Copyright ANSYS, Inc. All rights reserved.