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

ANSYS Mechanical- Shell and Link

  1. Sep 27, 2011 #1
    Hey guys,

    I am currently working on a project and need to model the tubing configuration as shown in the first attachment. Experimental testing has been completed and I have detailed data for the strain and vibration velocity as required.

    I need to model this in ANSYS to compare the results. To model the vibration shaker I need to model the rod as a spring with fixed support on the shaker side and a translation constrained in the axial direction on the tube side. I have used SHELL181 for the tubing and tried to use LINK180 for the rod as shown in the second attachment. However, when the mode shapes are calculated, the link doesn't behave as I would expect; the link isn't staying stiff causing a large deflection at the attached node and knocking out the frequency calculations.

    I'm not very experienced with this software but I think it should be relatively easy to fix. I just think the rod isn't being modelled properly. The only real constants I can use for the link are the area and I have chosen the rigid (classic) option. How can I adjust this?

    Any thoughts would be greatly appreciated, Cheers!
     

    Attached Files:

  2. jcsd
  3. Sep 27, 2011 #2
    If the link is just sharing a node with some elements on the pipe, then it'll be a non-physical point constraint, which might be causing too much deflection in the pipe wall. Are you seeing excessive deflection around that point, and in the pipe wall, rather than the link?
     
  4. Sep 27, 2011 #3
    Cheers for the reply.

    Yeah the link is just sharing the 1 node.
    If you have a look at the attached deformed shape for the first mode (12Hz), there is a huge deflection which I'm not happy with- this node shouldn't deflect that much, if any (rigid support). I tried solving the problem by modelling it as a fixed support at the node (lock all DOF's), but when I do a harmonic analysis, this node is also the point of force input which complicates things.

    Any thoughts?

    Also, is the nodal deflection (DMX) value scaled somehow?
    I don't understand why the value is 3.13 (i'm guessing metres).
    All the input parameters are SI units (m, kg, Pa etc) and clearly that deflection isn't consistent.... the total length of the tube is at most 0.6m.
     

    Attached Files:

  5. Sep 27, 2011 #4

    AlephZero

    User Avatar
    Science Advisor
    Homework Helper

    In this sort of modelling, normally you don't model the "stinger" rod from the shaker at all. After all, you really want to know the response of the pipe on its own, and if the stinger is affecting the response significantly, you need to change the test setup. (But so far as it's possible to tell from a picture, I think your test setup looks sensible).

    When you do a vibration analysis in a FE package, the amplitude of the each mode shape is arbitrary. Well, actually it is probably normalized to value that has nice mathematical properties, but that doesn't correspond to anything physical. If your plot of the mode shapes appear distorted because the amplitudes are too big, just scale them down when you make the plots.

    When you do the forced response analysis, make sure there is a mesh point on the pipe where you are applying the shaker. Then, just input a sinusoidal force at that point, along the direction of the stinger. To get the direction right, it may be easiest to define a local coordinate system at the grid point. (I've done plenty of FE dynamic analyses, but I don't use Ansys so I don't know in detail what input options are available)

    In the forced response analysis, the amplitude of the response will not be arbitrary. It corresponds to the force being applied through the shaker. So you should be able to compare the amplitudes in the model and the test directly. But remember than when you are close to a resonant frequency, the amplitude depends on the amount of damping you specify in the model, so you may have to adjust that, either by trial and error, or by doing a modal test on the structure to measure the damping.

    If you don't get any significant local distortion in the pipe where the stinger is applied when you do the test, you shouldn't be getting local distortions in the finite element model either. If you get local deflections because of the way you modelled the pipe with shell elements, you could try modeling it with beam elements instead.
     
  6. Sep 27, 2011 #5
    Is any of the deflection in the axial direction of the link element?

    That element has no stiffness to bending, so it will freely move in other directions. It has no rotational DOFs so they can't be constrained.
     
  7. Sep 28, 2011 #6
    OK Thanks, this is making me more confident with my results so far. The link element doesn't actually change things a great deal.

    I agree, the test setup is on the money and I believe that the strain/velocity data is quite accurate for the model. Thanks for clarifying in regards to the modal analysis, that makes perfect sense, I will just scale the plots down.

    By 'mesh point' do you simply mean an element node? If so, thats what I have done. In terms of defining the direction I just applied a 1N force in the direction of stinger.

    When I first ran the forced response analysis I calculated that maximum stress to be approximately 32MPa. However, from the strain data the calculated stress at this frequency was 0.18 MPa and I'm confident with this value. I used a trial damping ratio of 0.05, any ideas what's going on here as I'm fairly confident with the units?
     
  8. Sep 28, 2011 #7

    AlephZero

    User Avatar
    Science Advisor
    Homework Helper

    Yes. Different FE packages call them nodes, grid points, mesh points, etc. But "nodes" or "nodal points" can be confusing terminology in dynamics, where mode shapes also have nodes and antinodes.

    If the structure has a linear response (which should be a pretty good approximaition) then the stresss and strains you get will be proportional to the applied load.

    Are you measuring the load applied by the stinger? If the electrical system driving it is just an open-loop system controlling the voltage (i.e. there is no feedback loop using measured force in the stinger) the force applied to the structure may vary a lot with frequency, especially when you go through a reasonance of the system.

    IF you want to compare the detailed response of the model with the test (i.e. the complete shape of the frequency response, not just the location of the resonances) you need to measure the force in the stinger with a load cell between the shaker and the stinger rod. This will also give you the phase angle between the applied force and the displacement of the pipe, which will be close to 0 or 180 degrees when you are away from the resonant frequencies, but 90 degrees at the resonances.
     
  9. Sep 29, 2011 #8
    With the shaker tests we didn't actually measure the applied load, just the response signal from the strain gauges and accelerometers. I believe it was open-loop and it makes sense that this force would be amplified at resonance, and this was clearly visible in the pipe vibration during the test.

    However, for the purpose of this investigation I am interested in defining an allowable vibration velocity limit from the FE model. Using the linear relationship between stress and velocity and plotting it against frequency;

    Allowable velocity (f) [mm/s] = Endurance stress of material * RMS velocity (f) / Max Stress (f)

    As you can see, the calculated stress from ANSYS (derived from the input force arbitrarily selected as 1N) is scaled by the endurance stress. Using this method, the plots are very comparable and I have managed to determine that the measured velocity is less than the allowable velocity across the frequency range. This implies that the corresponding dynamic stress is less than the endurance stress and that failure won't occur.

    This aside, I am still having problems matching the natural frequencies in ANSYS to those measured in the testing. This I still put down to the stinger's effect.

    Do you think that this comparison is valid?
    Cheers for your time and help!
     
  10. Sep 29, 2011 #9

    AlephZero

    User Avatar
    Science Advisor
    Homework Helper

    Yup, getting the natural frequences to match between the model and the test is usually about 99% of the total problem :smile:

    I would expect the main cause of the difference is the way the structure is restrained, rather than because of the stinger. It's hard to see from your picture, but it looks like the bottom end of the pipe is fixed to something. That is unlikely to be the same as the perfectly rigid earthing in your FE model. You may get a better match by including some stiff springs in the FE model to simulate the flexibility of the clamp.

    There are two ways you could use to quantify this. One is to apply a static load to the pipe and measure its stiffness. The mass properties of your model are unlikely to be seriously wrong for a simple structure like a pipe, if you have checked that the total mass of the model equals the total mass of the pipe.

    The other is to do a modal test on the structure without the stinger. If you just want to check the frequencies, you only need to do a "bonk test" where apply and impulsive load (by hitting the structure with something), and do an FFT of the response. Of course with more sophisticated modal testing, you could measure the mode shapes, as well as the frequencies, but without knowing what background you have and what equipment is available, going into any more details is probably not very useful here.
     
Know someone interested in this topic? Share this thread via Reddit, Google+, Twitter, or Facebook