April 5, 2023 at 3:25 pmAlejandro FilgueiraSubscriber
I need to model a polymer (polypropylene) to perfom with it non-linear simulations (impact test, high deformation load status, etc...). The only information I have available to model the behaviour of this polypropylene is:
- Tensile Modulus: 1.100MPa
- Tensile Strain at Yield: 11 %
- Tensile Stress at Yield: 29 MPa
For the tests I need to consider both the elastic and the plastic behaviours of the plastic, because high deformations are expected.
Do you have any suggestion of what model should I use in Ansys Workbench and what specific values should I use for this modellization?
April 10, 2023 at 1:48 pmAshish KhemkaAnsys Employee
Please see if the following post helps you:
Material model for Polypropylene for impact simulation of box? (ansys.com)
April 11, 2023 at 9:07 amAlejandro FilgueiraSubscriber
I read that post but didn't give me enough information.
To begin with, I would need to be able to perform basic static tests with the plastic. So I am not sure Explicit Materials are the answer for this. I would need the way to describe an elastic behaviour with different parts: a linear part at the beginning and another area with a decrease in the slope of the stress-strain curve up to the 29MPa. How could I achieve this using Ansys Workbench?
April 11, 2023 at 1:59 pmArmin_ASubscriber
It looks like that you need a multi-linear elasticity model for your application. As far as I know, this model is not available via Workbench but it may be accessible via Mechanical APDL (MAPDL) commands. Please refer to the thread below where a similar topic was discussed:
Errors with Multilinear Elasticity material model (ansys.com)
April 25, 2023 at 8:28 amAlejandro FilgueiraSubscriber
I was able to phisically test the plastic and get a strain-stress curve. Is there any way in Workbench to model a material by entering these stain-stress points? As far as I have investigated I just have seen this possibiliy in the hyperelastic materials. Is there any other altenative?
April 25, 2023 at 1:47 pmArmin_ASubscriber
Do you see the bilinear elastic behavior in your experiment? If not, you can simply use a plasticity model within Ansys Workbench such as the "Multilinear Isotropic Hardening" to directly input the stress versus plastic strain curve into the model. Once you open Engineering Data, this model is available under "Plasticity" under the Toolbox.
April 28, 2023 at 11:41 amAlejandro FilgueiraSubscriber
Thanks Armin. But if I have raw strain-stress values in a chart, how can I separate the values that I have to input in the "Multilinear Isotropic Hardening" model? In this model the strain you have to input is the plastic strain, not the elastic one, right?
April 28, 2023 at 12:41 pmClaudio PedrazziSubscriber
Couldn't you simply subtract from each total (raw, measured) strain value the elastic strain, corresponding to yielding stress divided by E?
e_plast=e_tot - Sy/E
April 28, 2023 at 1:24 pmArmin_ASubscriber
What you obtained experimentally is likely engineering stress versus engineering strain curve. You should convert it to true stress versus true plastic strain before providing it to the model.
Please note that your resulting hardening curve should only be increasing with plastic strain, i.e., if your experimental data is noisy, an error message may appear when you solve the model. In such a case, it might be a good practice to fit a mathematical function (such as power-law or Voce functions) to your data so that it becomes smooth with true stress only increasing by plastic strain.
- 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.