General Mechanical

General Mechanical

Invalid Property data even after hyperplastic curve fit with Ogden

    • ayush_3
      Subscriber

      I am modelling a hyperelastic model for which I have the uniaxial tension and shear data. I did curve fitting with the Ogden 1st order material model, but it shows the following error when I ran the analysis:

    • peteroznewman
      Subscriber
      Don't leave the Incompressibility Parameter as 0. Calculate a value and use that. See this discussion.
      https://forum.ansys.com/discussion/20163/incomprehensibility-parameter-of-hyperelastic-material
    • ayush_3
      Subscriber
      Still, I am getting the same error; please see the figures below; if you need more information, I can give it.


    • peteroznewman
      Subscriber
      In Engineering Data, create a new material. Add Ogden 1st Order. Type in the three constants. In Mechanical, assign this new material to the solid body in the Geometry branch. Does it start working?
    • ayush_3
      Subscriber
      No sir, it didn't work. I have seen a lot of Youtube videos; they all do the same thing. There have to be some differences arising due to the version I am using, Ansys 2021 R1. There was a similar error due to the version settings, see my previous post on the Ansys forum here:
      I can't get to such errors all by myself, and I need your help.
      Please help.
    • peteroznewman
      Subscriber
      I opened one of my hyperelastic models using ANSYS 2021 R1 and did the steps described above and it worked for me. There much be something else wrong with your model. Please use File Archive to create a .wbpz archive and attach it to your reply. I will take a look.
    • ayush_3
      Subscriber
      That's so great of you sir, please see the file attached below.
    • peteroznewman
      Subscriber
      I immediately see why you get an invalid property error. You are using a Modal analysis. Modal analysis is a Linear analysis. No nonlinear properties are allowed in a Linear analysis. If you use a Static Structural analysis, you will see that this nonlinear material works fine.
      I noticed that your mesh is inadequate. It has only one solid element through the thickness. You should add Mesh controls to ensure at least 4 elements through the thickness. It is sometimes better to use Linear elements rather than Quadratic elements for Hyperelastic materials.
    • ayush_3
      Subscriber
      Sir, then is there no way to analyze the vibrational analysis with hyperelastic material properties? I have to apply the Triangular shocks, which were, I suppose, only possible through Random Vibrations for which Modal is a pre-requisite. And my project guide wants me to use the hyperelastic material.
    • peteroznewman
      Subscriber
      Please describe in detail the analysis you need to do. Describe in detail the "Triangular shocks" load.
      It is possible to apply a series of triangular profiles of acceleration vs time in a full Transient Structural model and obtain the transient response of the structure and use any nonlinear behavior you want such as contact, large deflection and hyperelastic material. No Modal analysis is required.
      If you have a linear system, you can use a Modal analysis and feed the modal results into the setup cell of a Transient Structural model to get a transient response in much less time than the full Transient Structural with no Modal.
      A train of triangular shocks is not a random vibration.
    • ayush_3
      Subscriber
      My shocks look like this:
      You can see a sharp increase in the acceleration in the first 5ms, then for another 5ms, it reduces to zero, then afterwards it is held constant at value 0.
      I want to apply this shock to my model with shock absorbers as hyperelastic materials.

    • peteroznewman
      Subscriber
      Okay. You can do that with a Transient Structural analysis. Just convert the g load to m/s^2 by multiplying by 9.8 and you can apply that load when the units are set to SI units.
      Make sure to include some damping in the simulation.
Viewing 11 reply threads
  • You must be logged in to reply to this topic.