General Mechanical

General Mechanical

Error with material failing in Non-Linear Analysis – Please help!

    • to2020
      Subscriber

      Hi,

      I am using the newer versions of ANSYS (19.1) and I have found the options to input the values in engineering data for the Menetrey William model.

      The following are the values I have inputted for Non-Linear Concrete.

    • John Doyle
      Ansys Employee
      I cannot look at your model, but I can offer a few suggestions.nYou might have tried this already, but if not below are a few tips to try as troubleshooting stepsn Switch all contacts to bonded.nTake out the Menetrey-Willam and run this with linear elastic properties.nWith the above two changes, model should converge. If it does not, there is something more fundamentally wrong with your setup (loads, BCs)nIf this test converges, add the Menetrey-Willam back into the model and keep all contact bonded. Also, try replacing the applied force with a displacement that produces the same reaction. This might be more stable.nIf that does not converge, try a separate model of just a simple block with just a few elements to test the Menetrey-Willam material model by itself under different modes of loading, just to gain understanding of how sensitive material model is to convergence under different modes of loading. From this exercise, if the material model input proves to be ok, try applying lessons learned (autotime stepping and solver specs) to the full model.nn
    • to2020
      Subscriber
      nPlease see the discussion above. The link in the discussion is no longer valid, hence use the link below to download the model: nhttps://unsw-my.sharepoint.com/:f:/g/personal/z5117866_ad_unsw_edu_au/EiAa1fHK7pZKtcZEuvpJXhsBxvc-hNutUS73igUNLX-5Iw?e=HORvo0 nThanks for your help in advance. n
    • peteroznewman
      Subscriber
      nHi Tony,ngave you some excellent suggestions, but when I open your link, there are old files from before that helpful reply. Please work on those suggestions and come back with new questions on these more controlled situations. Also, your file is over 1 GB in size. Delete the results and delete the mesh before saving and creating the archive to make the .wbpz file as small as possible.nI particularly like the idea of testing the material model on a simple block. I have done that with a single linear element, 8 nodes. Use 3 planes of symmetry so you have three orthogonal faces each with a zero normal displacement BC, leaving the other directions free. On a fourth face, apply a normal displacement of a known value of strain, again leaving the other directions free. Apply tensile strain in one analysis and compressive strain in another analysis to understand what the material model does in that one element. You will learn a lot. You can also apply a pressure to the fifth and six faces if you want to create a hydrostatic state of stress.nhttps://forum.ansys.com/discussion/1115/stress-strain-diagramn
Viewing 3 reply threads
  • You must be logged in to reply to this topic.