December 12, 2020 at 3:09 pmHarsihilZLHZSubscriberIf we want the Geometry/Part to behave within elastic limit, Why we consider Plasticity ?nAs soon as the equi Stress is greater than the yield Stress, then we can modify our Model to functional within Elastic limit.nIn one of ANSYS Course of Plasticity, they are comparing plastic strain from the experimental data to simulation, that I got it.nBut as we know that the Model has cross the yield Strength, then we can easily Modify Geometry/Part to behave within Elastic Limit. Hence my Question is , Why we need to Consider Strain hardening in the Simulation?.n
December 12, 2020 at 4:37 pmpeteroznewmanSubscribernYou don't need to add plasticity to the material model if the goal of the analysis is to evaluate the stress during the operational life of the structure and the requirement is to stay below yield. Just use a material model with linear elastic material properties.nThere are useful results plots to use in this evaluation. Insert the Stress Tool and choose max equivalent stress to get a Safety Factor plot or a Safety Margin plot.nOne reason to add plasticity is when there is a requirement that the structure does not collapse if a load that is four times the design load is applied. You may find that the maximum stress in the model at 4x Load with a linear elastic material has gone above the Ultimate Tensile Strength (UTS). In that case, you can't claim that the structure will pass the 4x Load test. nAdd plasticity to the material and solve the 4x Load model. In a Bilinear Hardening model with Tangent Modulus set to 0, that is known as an Elastic Perfectly Plastic (EPP) material and stress will never be above yield, so comparing to the UTS is pointless. The Safety Factor (or Safety Margin) to compute is to divide the Elongation at Break by the Total Strain (subtract 1 for the Margin). Elongation at break is a material property.nYou will likely find a small volume of the mesh goes plastic, but the surrounding material will remain elastic and support the 4x Load. However, if the whole section goes plastic, that predicts that the structure will collapse and not support the 4x Load. These models are generally run using Displacement BC and a Probe on that of the Reaction Force shows when the model passes the 4x Load point. In the case when the structure fails the 4x Load case, the reaction force will never reach that value, it will go up, flatten then go down before reaching the 4x Load value.n
- The topic ‘Why we consider Plasticity Model, if the target of the Geometry is to behave within Elastic limit?’ is closed to new replies.
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.
- How to do the frequency response of the nonlinear vibration of a flexible PCB?
- Importing Line and Solid Bodies from SpaceClaim to Mechanical
- how to open SendCommand in Ansys
- problems facing during solution
- Still facing the same issue
- Failed to move file from solver directory to scratch directory: file.rst
- Adaptive Sizing
- Stiffness factor
- Import DAT file
- Import pressure data (coordinates and value) to ansys workbench through excel
© 2023 Copyright ANSYS, Inc. All rights reserved.