April 9, 2023 at 9:44 pmJared McFaddenSubscriber
I am modeling a small section of an 8-strand mooring line with a force applied at one end and a fixed support at the other. The issue I am having is a high, unrealistic stress value near the face where the fixed support is applied, I think because of the fixed support. In the real application, there is not a fixed support at this end because it is just a small section of a much bigger line. I have tried both a fixed support and a displacement but both yield the same results ( I now realize that the two constraints do the same thing). The expected stress result should be similar to the probed value. Is there a better way to more accurately constrain this end?
April 9, 2023 at 10:18 pmpeteroznewmanSubscriber
The simple solution is to not plot the stress close to the fixed constraint. St. Venant's principle is that the stress far from a disturbance will be the same as the stress if there was no disturbance. There are two ways to only plot stress far from the distubance of the Fixed Support.
1. In Geometry
Use SpaceClaim to create a plane at the fixed end, then use the Move tool to offset it from the fixed end about 1-2 diameters of the line. Use Split Body to cut all the strands. On the Workbench tab, use the Share button to create Shared Topology so when the geometry is meshed, the elements share nodes at the cut boundary and no bonded contact is needed. Plot the stress on the bodies to the left and don't include bodies near the Fixed Support.
2. In Mechanical using Named Selections of Nodes
Create a Named Selection in the Worksheet of Nodes that have a Z coordinate > whatever value is needed, which will exclude all the nodes that have the artificially high stress. Plot the Stress using that Nodal Named Selection.
April 9, 2023 at 10:46 pmJared McFaddenSubscriber
Thank you very much for the response! I am using method 2 and have created a named selection that selected all nodes outisde of the artificially high stress. Is my next step to solve again and plot the stress? If so, the artificially high stress will be excluded?
I am also performing a fatigue analysis using the fatigue tool. Will this named selection method also exclude the high stress from the fatigue analysis?
April 9, 2023 at 11:18 pmpeteroznewmanSubscriber
You don't need to solve again. The artificially high stress is localized to the nodes near the fixed support but you ignore them and don't plot them and the values don't show up on the Legend of the plot using a Named Selection.
The same method should work on a Life plot using the Fatigue tool.
April 10, 2023 at 12:56 pmJared McFaddenSubscriber
I got it to work, thank you so much! Your comments to my post and many others' have helped me out immensely.
- 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.