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

to2020to2020 Member Posts: 37

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.


However, when I try to run the program, I keep getting error about how an element is failing. I am modelling the following pull-out test and using symmetry to only analyse half of it:




I have also used contact sizing and therefore the mesh for concrete near the rebar as well as the rebar has been set to 1mm (This is the smallest I could go for a 150mm diameter concrete cylinder with a height of 170mm on the Academic Version of Ansys).

I have applied the following analysis settings, boundary conditions and loading (force is corresponding to the yield strength of the bar i.e. 541MPa but only half of the load is applied due to symmetry):




I had to change it to unsymmetric solver type before as it would just won't run if I left it on program controlled.

I have attached the archive file to this post if someone is kind enough to take a look to see if I made any errors. I currently haven't defined a bilinear hardening model for steel as I was having errors running it when I defined it. But since I am only applying the load until yield strength, wouldn't specifying the yield strength be sufficient because it is still linear?

If someone could please help, it would be wonderful - it is for my thesis and I am new to this software!

https://unsw-my.sharepoint.com/:u:/g/personal/z5117866_ad_unsw_edu_au/EbxuvuDD7nBNl0403Sd8AtUBx4S1D9tSU63vP2W9WiJn3g?e=9vZgWD

Answers

  • jjdoylejjdoyle PittsburghMember Posts: 97

    I cannot look at your model, but I can offer a few suggestions.

    You might have tried this already, but if not below are a few tips to try as troubleshooting steps

    1. Switch all contacts to bonded.
    2. Take out the Menetrey-Willam and run this with linear elastic properties.

    With the above two changes, model should converge. If it does not, there is something more fundamentally wrong with your setup (loads, BCs)

    If 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.

    If 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.

  • to2020to2020 Member Posts: 37

    Hi @peteroznewman ,

    Please see the discussion above. The link in the discussion is no longer valid, hence use the link below to download the model:

    https://unsw-my.sharepoint.com/:f:/g/personal/z5117866_ad_unsw_edu_au/EiAa1fHK7pZKtcZEuvpJXhsBxvc-hNutUS73igUNLX-5Iw?e=HORvo0

    Thanks for your help in advance.

  • peteroznewmanpeteroznewman Member Posts: 11,072
    edited November 2020

    @to2020

    Hi Tony,

    @jjdoyle gave 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.

    I 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.

    https://forum.ansys.com/discussion/1115/stress-strain-diagram

Sign In or Register to comment.