November 18, 2022 at 8:08 pmAna Regina DehesaSubscriber
I'm fairly new to computational research, specially on Ansys. I'm working on my thesis project researching the artery damage that occurs during retrieval of a stent. My goal is to simulate this computationally on Ansys Static Structural. I have a long way to go, but I have gotten to the point where some external guidance would be very helpful.
At the moment, I'm basing myself off a couple tutorials, my model consists of a hollow cylinder (modeling the artery) with a solid rod inside of it (for now this is the "stent"). The inner diameter of the cylinder is 2.25 mm, outer diameter is 2.45 mm. The inner diameter of the hollow cylinder is exactly the same as the diameter of the rod, 2.25 mm (to make sure they are in contact). The length of both rod and cylinder is 20 mm. I changed the Operation parameter for creating the extrude to "Add Frozen" instead of "Add Material".
The material of the rod is simply stainless steel. The material of the hollow cylinder is a non-linear hypereleastic material (gotten from literature research of an artery's mechanical properties). I used the 5 parameter Moonley River model with the following specifications:
C10 = 0.0189 MPa; C01 = 0.00275 MPa; C20 = 0.59 MPa; C11 = 0.857 MPa; C02 = 0.015 MPa; D1 = 1.85 MPa^-1
I also added a density parameter from literature research of 1.13 kg m^-3.
There is a frictional contact between the rod's surface and the inner wall of the cylinder with a frictional coefficient of 0.3.
I turned Large Deflection on in Analysis Settings. I added Standard Earth Gravity in the appropriate direction.
I applied a Fixed Support to all of the faces of the hollow cylinder.
I created a displacement for all of the faces of the rod, in one single direction, to slide off the length of the hollow cylinder (20 mm) ("stent" exiting "artery").
I added to the solution equivalent stress and maximum principal stress for the hollow cylinder.
When I hit solve, the model runs, but there is barely any stress on the hollow cylinder. The max stress is 6.3e-10 MPa, and the minimum stress is -5.8e-10 MPa.
I'd like for the rod's displacement to exert a visible stress on the cylinder and right now that is not the case.
What could I add to the model to better reflect the stress exerted by the stent on the artery wall?
Any guidance is helpful! As you probably noticed I'm very much a beginner.
November 19, 2022 at 11:07 ampeteroznewmanSubscriber
Hello Ana Regina,
I expect the reason your model has very little stress in the artery is that there is no initial interference between the rod and the artery. The geometry was constructed with the same diameter for the rod and artery ID, so I am not surprised that there is no stress.
When a stent is expanded in an artery by a balloon, it stretches the artery. When the balloon deflates, the stretched artery applies a pressure to the stent, squeezing it. This is the state you need the model to be in before you start extracting the rod. There are several ways to put the model in that state.
The first way is to assign an initial state of stress on the artery. There is a command called INISTATE. This method is quite technical to implement, so let’s leave that aside for now.
A second way is to construct the geometry so that the stent (rod) diameter is larger than the ID of the artery. This would be a 2-step solution. In step 1, frictional contact between the artery and stent would be resolved. The contact algorithm would detect the interference and ramp up the contact force until the interference is driven to practically zero, stretching the artery in the process. In step 2, you pull the stent out of the artery. This can work for small values of interference.
The third way is to use a 2-step solution, but start with the geometry you have. In step 1, apply a thermal condition to raise the temperature on the rod, causing it to grow in diameter. The rod material will be given a Secant Coefficient of Thermal Expansion (CTE) material property using a number you will calculate to give the desired interference between the stent and the artery for the temperature load you apply. You can use orthotropic properties instead of isotropic properties so only the diameter gets larger, but the length doesn’t change because the CTE in the axial direction is 0. In step 1, the rod temperature increases by 1 degree C, the rod grows in diameter, stretching the artery. In step 2, the rod temperature stays the same and the stent is pulled out of the artery by the remote displacement.
In all these cases, delete the Fixed Supports from all the faces of the artery. You need a Remote Displacement, Behavior = Flexible, applied to the flat end face of the artery on the end opposite the direction the rod is being pulled. Set all six DOF to zero.
You also need a Remote Displacement, Behavior = Flexible on the flat end face of the rod on the end that is in the direction the rod will be pulled. Set five DOF to zero, leaving the axial direction Free. Promote that Remote Displacement to a Remote Point. Apply another Remote Displacement, but scope it to the Remote Point you just created. This Remote Displacement has a Tabular input for the 2-step solution. The axial displacement is 0 in step 1, which holds the rod in place while the artery expands in step 1. The pull distance is applied in step 2.
For this initial simple model, I suggest you make the rod longer than the artery. Edit the geometry of the rod and put a generous blend radius on the sharp edge at the end face. The reason is that as the rod is removed, the artery, which is stretched over the rod, will want to contract to its original diameter. It will be numerically very difficult for the nodes of the artery to slide off a sharp edge of the rod. Make that end of the rod have a dome shape, or at least a blend that leaves a very small flat.
I hope that gets you started. I will check back for any follow-up questions.
- 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.