March 4, 2023 at 4:56 pm
March 4, 2023 at 6:03 pmpeteroznewmanSubscriber
It may be the mesh is not connected. You can confirm this by dropping a Modal analysis on the Model cell of Static Structural in Workbench then in Mechanical, drag the Fixed Support down and drop it on the Modal branch. In Analysis Settings for Modal, request 12 modes and Solve. If you find the first 6 modes are practically zero, you have an unconnected mesh. Set the display displacement scale factor to 0 and use the Total Deformation plot to see where the connection is broken. Or the animation might also show you where it is broken.
Try to use the Mesh Merge command to merge two coincident nodes so that a connection is established.
March 4, 2023 at 10:04 pmHoang NGUYENSubscriber
Yes, the mesh was not conencted i have used node merge to fix the problem. Thank you so much. I want to ask one more question: how can i apply pressure on the external face of this cylinder. This is a line model so i can't choose the external face to apply pressure. I'm thinking using the line pressure but i dont know if it will apply to all the model not just the external face and i can't manage to have a normal pressure with line pressure. Can you help me with this problem?
March 4, 2023 at 10:36 pmpeteroznewmanSubscriber
Instead of applying a pressure, you could create a cylindrical surface (tube) around the wire structure, and add frictional contact between the surface and the wire. You would delete the Fixed Support on the wire structure. You could apply a radial displacement to the nodes on the tube that would shrink the diameter of the tube. You could apply a Thermal Condition to the elements on the tube that would shrink the tube. If you apply an Orthotropic Secant Coefficient of Thermal Expansion so that it only shrinks in one direction, which would be the tangential direction in a cylindrical coordinate system. You would need to apply this coordinate system to the elements on the tube.
March 5, 2023 at 10:02 amHoang NGUYENSubscriber
I want to know for each pressure given applied on the external wall, how the model will be moved and deformed. Can i do that by create a tube around the structure?
If yes, can you show me how can i do it? I will create it in Geometry or in Model?
Thank you so much
March 5, 2023 at 12:10 pmpeteroznewmanSubscriber
After a stent is made, a balloon is inserted into the center. The stent begins at a diameter smaller than the constricted artery that needs to be treated. Once placed at the site of the constriction, the balloon is inflated which pushes on the stent and the artery to expand the diameter of the stent and artery. The balloon is deflated and removed, but the expanded stent remains to hold the artery open at a new larger diameter because the stent was plastically deformed.
I have seen models that apply pressure on the inside of a stent to expand it. The pressure is simulating the pressure in the balloon.
I have seen models that include an artery for the stent to press against. The elastic property of the artery pushes back against the stent as the artery is stretched open.
The tube I described in my last reply could represent the balloon if it was inside the stent, pushing out. You could apply pressure instead of displacement and that would be a good simulation of the balloon expansion phase of stent deployment.
I’m confused why you want to apply pressure on the outside of the stent pushing in. That doesn’t match any part of the process that I am aware of.
I suppose you could apply an inward pressure to the tube on the outside of the stent, but the issue would be the wrinkling and folding of the tube as it shrinks. That doesn’t happen when you inflate a balloon and the material stretches as it expands.
- 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.