1. Limited time only! Sign up for a free 30min personal tutor trial with Chegg Tutors
    Dismiss Notice
Dismiss Notice
Join Physics Forums Today!
The friendliest, high quality science and math community on the planet! Everyone who loves science is here!

ANSYS workbench - finer elements gives errous results

  1. Apr 16, 2010 #1
    Hello!

    I'm doing a simulation in ansys workbench mechanical (12.1) of a cantilever beam (axle) fixed to a wall and loaded radialy at the other end.

    The funny thing here is that when the mesh is rather coarse the results regarding von-mises stress (at the support where the bending moment is at it's highest) is very accurate compared to the theoretical values. When the mesh is getting finer, the results gets higher and higher and deviates from the theoretical ones.

    the opposite happens with the total deformation where the results are getting more and more correct as the elements are getting finer and finer.

    Does anyone have a reasonable explanation to this?

    thanks
    Frode
     
  2. jcsd
  3. Apr 16, 2010 #2
    The fact that you refine the mesh and the stresses skyrocket indicates a stress singularity probably close to a constraint point. Deflections are small (as it's constrained) mean that you would expect to see the displacement not change much at that end.

    I thought ansys workbench had adaptive meshing. If you have this on, turn it off and do a standard mesh. If you have it off, turn it on and see what happens.

    How far from calculated values are you?

    Check your constraints, one that doesnt truly reflect the load case you are thinking of can cause funny results. eg something like a fixed constraint where it should be compressive only (I know this doesn't directly apply but you get the idea - check your loading conditions).

    As far as I remember you have very little control over element type in workbench, so I doubt that is the issue.
     
  4. Apr 16, 2010 #3
    I found that adaptive meshing is not an option for my mechanical workbench I'we found out.

    See the atached image for details.
    I've used fixed support and the load is applied at the face as force with 10000N in magnitude.

    Also, what is the consequence of using element midside nodes regarding the results?
     

    Attached Files:

  5. Apr 16, 2010 #4
    It's accurate to approx 1%... Thats pretty damn good. when I do FEA simulations (granted they are more tricky than this and are harder to validate) but 5% variation is deemed acceptable.

    Midside nodes allows the element to take on a curved edge. Allowing better fidelity to round objects with less elements.

    Read up on H-refinement and P-refinement.
     
  6. Apr 16, 2010 #5

    minger

    User Avatar
    Science Advisor

    Firstly, what kind of elements are you using? If you are using SOLID elements, then you'll have a discontinuity as Chris suggested at the "wall" (I assume that you're not actually modeling the wall, as indicated by the images).

    Again, as Chris suggested, with solid elements on an analysis such as this, 1% error is pretty good. However, you can try using BEAM elements, they should actually give better results for this particular problem.

    edit: I'm not sure that Workbench has an adaptive mesher, however what is now called ANSYS APDL does. There is a command called....ADAPT maybe that you can issue during the solution environment to allow the solver to refine the mesh based on the results.

    p.s. I'm not 100% sure about the ADAPT command (I no longer have access to the ANSYS help files).
     
Know someone interested in this topic? Share this thread via Reddit, Google+, Twitter, or Facebook




Similar Discussions: ANSYS workbench - finer elements gives errous results
  1. Proper ANSYS Element? (Replies: 12)

Loading...