Dismiss Notice
Join Physics Forums Today!
The friendliest, high quality science and math community on the planet! Everyone who loves science is here!

Stress convergence, Ansys

  1. Dec 25, 2013 #1
    Hi,

    I am trying to model a simple plane stress problem using Ansys. I am using Ansys 14.0.
    The problem is a simple square plate, with out a corner, and with a hexagon hole around the midle. The boundary conditions consist of a constant pressure on the top side, and full constrain on the bottom.

    In order to study the convergence, I listed the maximum displacements and stress on the entire domain. I realized that the displacements converged fairly good. However none of the stresses, namely [itex]\sigma_{x}[/itex], [itex]\sigma_{y}[/itex] and [itex]\sigma_{xy}[/itex], converge. You can see on the attached image, how bad the situation is. I don't know exactly why is this happening.
    On the attached image I have ploted the converge study for the [itex]\sigma_{x}[/itex] stress only. Note that on the last mesh, I used a mesh 5 times finer that the previous one. Also, the last meshes are highly dense. In fact the 5th mesh from the bottom already corresponds to 50 elements on the right side.

    also,

    The thickness is around 0.01 [m].
    I used plane182 elements, with element behaviour selected as plane stress with thickness.

    Any help is appreciated,
     

    Attached Files:

  2. jcsd
  3. Dec 26, 2013 #2
    Just guessing here, but what is the radius on the corners of the hexagonal hole? Can you plot the results up to where you stop the analysis (or it stopped itself), and see where it's diverging?
     
  4. Dec 26, 2013 #3
    The radius is 0.008[m]. It is a regular hexagon.

    The analysis runs all the way. And pretty fast too.(except for the last mesh)
     
  5. Dec 26, 2013 #4

    AlephZero

    User Avatar
    Science Advisor
    Homework Helper

    Dawin means the fillet radii at the 6 corners of your hexagon. In your picture, it looks as if the hexagon is 6 straight lines meeting at angles of 120 degrees.

    If that is the case, the stresses won't "converge", because the mathematical solution says the stress is infinite at the sharp corners.

    Of course in real life, the corners are not perfectly sharp, most structural materials (e.g. metals or plastics) will yield in a small region at the corner, and for metals the material is not probably not even isotropic at length scales of the same order as the grain size.

    The way to deal with all that "in real life" is find the stress levels around the hole ignoring the local stress concentrations, and then apply a stress concentration factor from a book like http://www.amazon.co.uk/Petersons-Stress-Concentration-Factors-Walter/dp/0470048247
     
  6. Mar 16, 2014 #5
    Forgot to thank you at the time. Your answer was helpful.
     
Know someone interested in this topic? Share this thread via Reddit, Google+, Twitter, or Facebook




Similar Discussions: Stress convergence, Ansys
Loading...