TAGGED: error, mechanical
May 23, 2023 at 4:07 amJia-Wei LiaoSubscriber
Hello, I'm currently working on breast compression simulation. The simulation is moving the upper board downward to compress the breasts. Here is a some images for reference.
The boundary conditions are set as follows
The geometry of breast as shown in the image below
The material properties are using the Mooney-Rivlin model, and the values are obtained from the paper.
The mesh I use linear hexahedron and element size I use 1 mm , it can get 425681 nodes and 598742 element. And the average element quality is 0.77688.
The goal is to move the upper board downward by 100mm to compress the breast. The simulation is divided into multiple steps, with each step moving the board downward by only 1mm. However, when upper board downward by 84mm, a high distortion issue occurs, as shown in the image below.
After the error occurred, I checked the residual force and found that there were no issues in other areas except for the initial contact surface between the breast and the upper board. Convergence issues were observed, and the mesh dostortion can also be seen, as shown in the image below.
I have already tried change element type into tetrahedron and add a nonlinear adaptive region, or decreasing the displacement values at each step, but it still cannot achieve convergence. I would like to know if there are any other ways to solve this error?
May 23, 2023 at 6:06 amNanda VerallaAnsys Employee
Hyperelastic materials such as rubbers are used in a variety of engineering applications for sealing and other purposes. In many of these applications, the components made of hyperelastic materials experience large strains, and modeling such cases often involves accounting for geometric, material and contact nonlinearities. Due to these reasons, we often encounter the excessive element distortion error when using hyperelastic materials in our simulation. In this video, experts discuss why element distortion errors occur and you get to learn how to understand various error messages and use them to diagnose and fix the underlying issues.
How to Handle Element Distortion Errors in Hyperelastic Materials — Lesson 3 – ANSYS Innovation Courses
Let me know if this doesn’t help.
Guidelines for Posting on Ansys Learning Forum
How to access ANSYS help links
May 23, 2023 at 7:14 amJia-Wei LiaoSubscriber
Thanks for your reply!
This video is helpful to me, but I have tried all the methods mentioned in it, but I still can’t solve the problem of highly distorted. I would like to ask if there are other ways to solve the problem of highly distorted? If the material property is changed to linear Is elastic better?
May 23, 2023 at 7:40 amNanda VerallaAnsys Employee
could you make the following changes and run the solution.
- Change the contact settings between displacement plate and your model
- Normal stiffness-->Factor, Normal stiffness factor-->0.1
- Detection method-->Combined
All the best,
May 23, 2023 at 7:52 amJia-Wei LiaoSubscriber
Thanks for your reply!
I will change the contact setting and run the solution again.
I want to ask a question.
Contact settings between displacement plate and model-->Interface treatment，if i set "adjust to touch" is ok? or "add offset,ramped effect" is better? or there are another suggestions?
thanks you very much
May 23, 2023 at 9:57 amNanda VerallaAnsys Employee
That really depends on model and your initial contact status, using contact status information, your selection for the Interface Treatment property can improve the contact status from Far Open or Near Open to Closed. Having a Contact Region in Closed status at the beginning of the analysis may improve the convergence of the model.
- Adjust to Touch: Any initial gaps are closed and any initial penetration is ignored creating an initial stress free state. Contact pairs are "just touching" as illustrated.
Add Offset, Ramped Effects: Models the true contact gap/penetration plus adds in any user defined offset values. Using this setting will not close gaps. Even a slight gap may cause bodies to fly apart. Should this occur, use a small contact offset to bring the bodies into initial contact.
To know more about geometric modification, please refer to this link below:
Geometric Modification (ansys.com)
May 24, 2023 at 3:59 amJia-Wei LiaoSubscriber
Thanks for your reply!Your advice is really importantI also want to ask a question about meshWhen it is suggested to use hyperelastic materials in the above video, it would be ideal to use linear for element order, but I have seen other websites saying that it would be better to use quadratic. Based on your experience, do you think that using hyperelastic materials and perform large deformation simulation, is it better to use linear or quadratic element order?
thanks you very much
May 24, 2023 at 6:55 amNanda VerallaAnsys Employee
As you are aware, linear elements lack midside nodes, while quadratic elements do have those. When quadratic elements are significantly deformed, the midside nodes are displaced, and these displaced locations may occasionally cause the edges on which they are located to bend sharply, or they may cross through the domain of the element and enter a face on the other side. Because linear elements lack the midside nodes that may cause severe element distortion, a linear mesh is frequently more resistant to "mesh entanglement" than a quadratic one. Here is an Ansys help link, giving further insights on linear and quadratic elements.
2.2. Choosing Between Linear and Higher Order Elements (ansys.com)
- 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.