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

ANSYS Modal: What does the deflection result represent?

  1. Dec 12, 2013 #1
    I was told in a meeting, in passing, not to pay any attention to the deflection results that come out of a free vibration problem. Can someone clarify why or point me to a good resource where I can inform myself?

    Thanks,
    KC
     
  2. jcsd
  3. Dec 12, 2013 #2

    AlephZero

    User Avatar
    Science Advisor
    Homework Helper

    You should certainly pay attention to the shape of the deflections (i.e. the "mode shape"), but the amplitude you get from a free vibration model is arbitrary.

    In real life, the amplitude depends on the forces applied to the structure, but a vibration analysis ignores the forces and just tells you what modes of vibration could occur, and at what frequencies, not what modes will occur.

    The shapes are important, because if you apply the same level of force to the structure, it will create bigger vibration amplitude when it is applied at the positions which move most. (The basic reason is that the force transfers energy into the vibrating object be doing work, and work = force x distance, so more distance means more work).
     
  4. Dec 13, 2013 #3
    Thanks for that AlephZero. That's kind of what I was thinking. It's the relative deflections that give you insight. I am guessing that it only makes sense to look at relative deflections within a given mode shape? For example, would it be meaningful to compare the deflection of the endpoint of a cantilevered beam at mode 1 to the deflection at any other mode?

    I guess if I had a better idea of how ANSYS is actually making the calculations, I could answer that on my own.
     
  5. Dec 13, 2013 #4

    AlephZero

    User Avatar
    Science Advisor
    Homework Helper

    The simple-minded answer is, you can only compare the relative deflections at different points in the same mode shape. You can't compare the size of the deflections at the same point in two different modes - unless the deflection is zero at that point in one of the modes.

    The less-simple-minded answer is, it depends how the different mode shapes are "normalized" when they are output. There are two "common sense" methods that are sometimes used:

    1. Make the biggest deflection in each mode = 1.0 (wherever it occurs, usually at a different place in each mode)
    2. Make the deflection at a place that you specify in the input = 1.0, for all the modes. (The deflection at other places in the structure maybe bigger than 1, of course).

    But more likely, the mode shapes will be "mass normalized", which means the product ##x^TMx = 1## where ##x## is the mode shape vector and ##M## is the mass matrix of the structure. That means the internal energy (potential + kinetic) in different modes is proportional to the frequency squared, for the values of the displacements that are output.

    The reason for this choice is because it is very convenient for using the mode shapes as generalized coordinates (in the sense of Lagrangian mechanics) for dynamic analysis both in the time domain (transient dynamics analysis) and the frequency domain (steady state response analysis). Most course notes / web sites / textbooks on dynamics of multi degree of freedom (MDOF) systems will have some of the math behind this, for "simple" systems modeled by point masses connected by springs. The basic ideas are exactly the same for finite element models - the only difference is that the finite element mass and stiffness are formulated in a more general way.
     
    Last edited: Dec 13, 2013
Know someone interested in this topic? Share this thread via Reddit, Google+, Twitter, or Facebook




Similar Discussions: ANSYS Modal: What does the deflection result represent?
Loading...