July 7, 2020 at 3:06 pmStatSubscriber
Hello everyone, I am trying to simulate a stent expansion inside an artery. When I expand just the balloon (simulated as a cylinder) inside the artery there appears no convergence issue (image 1). However when the stent is also introduced, the solution fails to converge without reasoning in the solver output (image 2). Are there any recommendations? Feel free to ask me any questions regarding my model.
July 7, 2020 at 4:22 pmWenlongAnsys Employee
Have you tried balloon and stent only (without artery)? That can probably give you insight into the possible reason for this non-convergence.
July 7, 2020 at 4:51 pm
July 7, 2020 at 5:00 pmpeteroznewmanSubscriber
I expect the extra edges of the stent pressing on the artery cause convergence issues.
One strategy is to soften the contact between the stent and the artery, relaxing slightly the penetration tolerance.
July 7, 2020 at 5:24 pm
July 7, 2020 at 5:57 pmWenlongAnsys Employee
If you right-click on "Solution information" --> Insert --> Contact, you can create a contact tracker and find out the current penetration in your model. You can adjust based on that value.
In case you are using asymmetric contact, it will be a good idea to set the artery as the contact surface because its stiffness is much lower than the stent. At the same time, make sure the mesh in the artery in the contact area is small enough to capture contact behavior. As Peteroznewman mentioned, you can try a lower normal stiffness factor, such as 0.1
You can also define multiple steps to help improve efficiency. For example, in the first step, you can define the B.C so that the stent almost contacts the artery, and in the second step, the contact between them starts. In this way, you can have fewer substeps in step 1, since no convergence difficulty is involved. This way it can save some computational time.
July 7, 2020 at 8:45 pmpeteroznewmanSubscriber
As Wenlong says, soften the contact stiffness by using the Normal Stiffness Factor and a good first try is 0.1
July 17, 2020 at 8:53 amStatSubscriber
Since I am investigating the structural integrity of the stent, I don't need a dense mesh for the whole artery, because computational time increases dramatically.
Is there a way to create a thin layer of dense mesh at the contact areas between the stent and the artery, while maintaining the rest of the mesh intact?
July 17, 2020 at 2:09 pmWenlongAnsys Employee
You can try "inflation" when you do the mesh. (https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/wb_msh/ds_Inflation.html)
But be careful the element aspect ratio in the inflation region should be close to 1 (in other words, don't make the element too thin in the inflation region compared to its other two dimensions).
Also refer to :
July 21, 2020 at 10:15 amStatSubscriber
Inflation method works but without the Hex dominant method. I guess there is no way those two can coexist right?
July 21, 2020 at 12:09 pmpeteroznewmanSubscriber
Correct, it is one or the other. They are exclusive.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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 calculate the residual stress on a coating by Vickers indentation?
- An Unknown error occurred during solution. Check the Solver Output…..
- Saving & sharing of Working project files in .wbpz format
- Solver Pivot Warning in Beam Element Model
- Understanding Force Convergence Solution Output
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- Massive amount of memory (RAM) required for solve
- What is the difference between bonded contact region and fixed joint
© 2022 Copyright ANSYS, Inc. All rights reserved.