General Mechanical

General Mechanical

Stent deployment

    • Stat
      Subscriber

      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.



    • Wenlong
      Ansys Employee

      Hi Stat,


      Have you tried balloon and stent only (without artery)? That can probably give you insight into the possible reason for this non-convergence. 


      Regards,


      Wenlong


       

    • Stat
      Subscriber

      I appreciate the quick response sir!


      Yes I have tried to deploy the stent alone and the solution converged succesfully with the subsequent result.



      Kind regards,


      Stathis

    • peteroznewman
      Subscriber

      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.

    • Stat
      Subscriber

      Thank you for the suggestion sir!


      So are you proposing to increase the penetration tolerance value? If this is the case, what value would you recommend?


      To provide some perspective, the stents thickness is 0.08mm and its element sizing 0.05 mm.


      Kind regards,


      Stathis

    • Wenlong
      Ansys Employee

      Hi Stathis,


      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. 


      Regards,


      Wenlong

    • peteroznewman
      Subscriber

      As Wenlong says, soften the contact stiffness by using the Normal Stiffness Factor and a good first try is 0.1

    • Stat
      Subscriber

      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?

    • Wenlong
      Ansys Employee

      Hi Stat,


      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 : 


      Regards,


      Wenlong


       

    • Stat
      Subscriber

      Inflation method works but without the Hex dominant method. I guess there is no way those two can coexist right?

    • peteroznewman
      Subscriber

      Correct, it is one or the other. They are exclusive.

Viewing 10 reply threads
  • You must be logged in to reply to this topic.