Skip to main content
G
GavinBRumble10-Marble
10-Marble
June 6, 2006
Question

Vibration is not an option

  • June 6, 2006
  • 6 replies
  • 1517 views
Okay, bad choice of words, but lingo or terminology is exactly the point of this message. After hours pouring over the Help files, Verification models, etc., I'm no closer to being comfortable with the Dynamic Analysis (Structure) interface. This seems like a simple problem:
A large structure (vibratory conveyor) is vibrating due to an eccentric driver mounted on a motor (these things are fairly common on vibratory feeders). I am going to be bolting my device to the structure and want to check out the response...look for weaknesses.
Speed: 900 RPM so Frequency is 15 Hz
Amplitude: +/-.125" at 15 degrees from vertical

This seems like a Base Excitation loading, but the UI baffles me. It may be that there is more than one way to skin this cat, but if you know of one I'd love to hear about it. I'd like to be able to run the 15 Hz against several iterations to determine response, as well as graph the system response to speeds ranging from 10 to 20 Hz.

Thanks,

Gavin B. Rumble PE
Solid Engineering

    6 replies

    G
    GavinBRumble10-MarbleAuthor
    10-Marble
    June 6, 2006
    Suggestions were to run a Dyn Tme study. But it is the loading UI that is
    confusing. What are the units of the results of a custom function you would
    enter for Dyn Time Base Excitation for example? "Help" says that Base
    Excitation acts thru the constraints. So surely the units cannot be lbs
    (force)...a force acting at a constraint is always a no-no, or at least
    ignored. Same question for Dyn Freq Base Excitation...what are the units?

    I did place a Support call. The nice young man pointed us to the Help files
    and said he couldn't do any consulting...which is understandable IF THE HELP
    FILES ARE COMPLETE AND UNDERSTANDABLE. He did say Mechanica DOES NOT
    support Enforced Dynamic Displacement. This sounds like the problem I want
    to run...should I hire an ANSYS guy?

    Thanks in advance,

    Gavin B. Rumble, PE
    Solid Engineering
    336-224-2312



    Original Replies:
    ---
    David - Maybe you can run a Dynamic Time analysis that will show you the
    transient response. After a while it will settle down into a steady state
    response. No point in taking it further than that.

    Or if you have varying frequency then you're looking at a Dynamic Frequency
    analysis.

    The key is getting your measures set up right. Getting your input right is
    (as you're discovering) quite hard too.

    Run your first analysis just looking at measures (I prefer 'relative to
    supports') then run again, requesting 'full results' at specific points of
    interest - i.e. peaks of measures on graphs etc.
    ---
    Jeff - One of the types of analyses (not Dynamic Random....maybe it's
    Dynamic Frequency?) allows you to input a repeating function as the
    vibration input.

    You need to first run a static analysis (if there are static loads), then
    run a modal analysis, then run the final Dynamic Frequency(?) analysis. Log
    a call to Tech support; perhaps they'll fill in some more information for
    you.
    ---

    Original Question:

    Okay, bad choice of words, but lingo or terminology is exactly the point of
    this message. After hours pouring over the Help files, Verification models,
    etc., I'm no closer to being comfortable with the Dynamic Analysis
    (Structure) interface. This seems like a simple problem:
    A large structure (vibratory conveyor) is vibrating due to an eccentric
    driver mounted on a motor (these things are fairly common on vibratory
    feeders). I am going to be bolting my device to the structure and want to
    check out the response...look for weaknesses.
    Speed: 900 RPM so Frequency is 15 Hz
    Amplitude: +/-.125" at 15 degrees from vertical

    This seems like a Base Excitation loading, but the UI baffles me. It may be
    that there is more than one way to skin this cat, but if you know of one I'd
    love to hear about it. I'd like to be able to run the 15 Hz against several
    iterations to determine response, as well as graph the system response to
    speeds ranging from 10 to 20 Hz.
    I
    iapanovitch1-Visitor
    1-Visitor
    June 7, 2006
    Gavin,

    1. It looks like you should run Frequency response -- range from 10Hz to 20Hz, just make sure you have 15Hz (0.5 interval between 10 and 20Hz) requested in Output tab. Then you'll have 2 rabbits shot with 1 bullet (as a Russian saying goes...) -- get full results at 15Hz, as well as get the system's response from 10 to 20Hz.

    2. Base excitation in Pro/M is defined as acceleration, so you should calculate the acceleration amplitude of the 'base' (pretty trivial task since you know the displacement amplitude and frequency) in whatever units you use for your model (e.g. m/s2, or in/s2, etc) -- given your desciption of the system, it looks like you should end up with a 'parabolic' acceleration amplitude function (i.e. acceleration proportional to frequency squared) -- then enter this function in the analysis definition form.

    Hope it'll be of some help, and -- good luck.

    Yuri, Ph.D,P.Eng.
    I
    iapanovitch1-Visitor
    1-Visitor
    June 7, 2006
    P.S. While I remember... Since you'll be running base excitation, use mass participation factors to ensure the accuracy of your analysis. The total should be 0.8 or greater (0.9 or greater, I believe, is required by US Navy in their shock analysis requirements...), otherwise you'll need to use more modes (determined in the Modal analysis used for the Dynamics).

    Yuri
    U
    unknown11-Visitor
    1-Visitor
    June 7, 2006
    Thank you all for the comments...this is starting to make some sense (in
    other words, I'm just realizing more that I don't yet understand...is that
    progress?). I'll post a summary sooner or later, but first I may pose a few
    more questions.

    I think when the "No Dynamic Enforced Displacement" limitation of
    Pro/Mechanica finally sinks into my feeble brain we will start to get closer
    to the solution...we were trying so hard to make THAT work! I think we are
    starting to get our arms around the idea of an accel input instead of a
    displacement input...it is, after all, just the 2nd derivative of
    displacement (as a function of time). Part of the problem is they (the PTC
    developers) left off the Acceleration label in the function UI for Base
    Excitation Frequency studies...a person has no idea what quantity the
    function is calculating!

    Regards,

    Gavin


    Original Question:

    Okay, bad choice of words, but lingo or terminology is exactly the point of
    this message. After hours pouring over the Help files, Verification models,
    etc., I'm no closer to being comfortable with the Dynamic Analysis
    (Structure) interface. This seems like a simple problem:
    A large structure (vibratory conveyor) is vibrating due to an eccentric
    driver mounted on a motor (these things are fairly common on vibratory
    feeders). I am going to be bolting my device to the structure and want to
    check out the response...look for weaknesses.
    Speed: 900 RPM so Frequency is 15 Hz
    Amplitude: +/-.125" at 15 degrees from vertical

    This seems like a Base Excitation loading, but the UI baffles me. It may be
    that there is more than one way to skin this cat, but if you know of one I'd
    love to hear about it. I'd like to be able to run the 15 Hz against several
    iterations to determine response, as well as graph the system response to
    speeds ranging from 10 to 20 Hz.
    U
    unknown11-Visitor
    1-Visitor
    June 13, 2006
    Several great suggestions were mentioned (summarized below) but this simple
    problem is wupping us. Neither the Stiff Spring method of Enforced
    Displacement or the Base Excitation method are returning expected results.
    Either we are expecting the wrong thing, doing it all wrong, or Mechanica is
    broke and needs fixing.

    See this webpage for a description of the problem with screen shots.
    http://www.solidpe.com/BaseExcitation.htm

    First, using the Stiff Spring method recommended by Mr. Holst we were
    getting enforced displacements of 0.0025 inches with 125 lbf acting at a
    1000 lb/in spring...way short of the 1/8" that that force should have
    produced. Besides, the harmonic (16.xx Hz) of the ruler itself was showing
    up in the (spring mounted) base even though the spring is way stiffer than
    the ruler.

    Second, the Base excitation is returning screwy Base Displacements (see
    webpage above).

    As Bill O'Reilly says, "Where am I going wrong...?"

    SUMMARY:
    === Yuri ===
    1. It looks like you should run Frequency response -- range from 10Hz to
    20Hz, just make sure you have 15Hz (0.5 interval between 10 and 20Hz)
    requested in Output tab. Then you'll have 2 rabbits shot with 1 bullet (as a
    Russian saying goes...) -- get full results at 15Hz, as well as get the
    system's response from 10 to 20Hz.

    2. Base excitation in Pro/M is defined as acceleration, so you should
    calculate the acceleration amplitude of the 'base' (pretty trivial task
    since you know the displacement amplitude and frequency) in whatever units
    you use for your model (e.g. m/s2, or in/s2, etc) -- given your desciption
    of the system, it looks like you should end up with a 'parabolic'
    acceleration amplitude function (i.e. acceleration proportional to frequency
    squared) -- then enter this function in the analysis definition form.

    3. Since you'll be running base excitation, use mass participation factors
    to ensure the accuracy of your analysis. The total should be 0.8 or greater
    (0.9 or greater, I believe, is required by US Navy in their shock analysis
    requirements...), otherwise you'll need to use more modes (determined in the
    Modal analysis used for the Dynamics).

    === Jim ===
    I don't know if it helps or if useful, but I show a method for doing
    Enforced Dynamic Displacements in the Tips&Tricks section of my web site.
    www.TSDengineering.com

    === David ===
    1. Base Excitation is precisely putting your acceleration inputs at the
    constraints. And as we all know Force and acceleration are related when
    mass is involved. Think of it like being an earthquake. Normally you
    constrain the base and it's rock solid, but then that solid base itself gets
    wiggled. Your option is either to do base excitation (vibrating the
    constraints) or to oscillate an applied load. So you can'y apply an
    enforced displacement and oscillate that (Not to my knowledge at least).

    === Rami ===
    I'm not entirely sure that you need to use vibration analysis in mechanica.
    According to your description, at least as I understood it, you better use
    MDX (mechanism analysis). The beauty of it is that after you have calculated
    what you need/want in MDX you can transfer it directly into mechanica
    (structural).
    The vibration analysis in mechanica is great for detecting small deflection
    inside the model or an assembly, however I found that MDX is better & easier
    for the rest. Now since you know your input I don't think you will have any
    difficulties.

    END OF SUMMARY

    Regards,

    Gavin
    U
    unknown11-Visitor
    1-Visitor
    June 13, 2006
    Dear Gavin,

    Looks like Mechanica's working OK to me from the info on your web-page.

    disp = a sin(wt)
    velo = aw cos(wt)
    accel = -aw^2sin(wt)

    So if a = 0.125", then the peak velocity will be 11.78 inch/sec, and peak
    acceleration 1110.3 inch/sec^2 at 15 Hz. You haven't multiplied w^2 by the
    displacement, so your acceleration input is 8 times too high.

    You will notice that the velocity is a cosine function, thus there is an
    initial velocity of 11.78 inch/sec. For your Mechanica input the initial
    velocity would be 94.24 inch/sec, or 37.7 inch in 0.4 seconds. This is
    what your second graph shows, hence Mechanica is doing the calculations
    correctly.

    What you need to do to get the 'correct' results is to select 'relative to
    supports' in the dynamic time analysis dialog box, then you will get the
    results that you expect.

    If you're ever in the UK, you could consider taking our Advanced Mechanica
    Vibration course!

    Regards,

    Rod Giles
    Mechanica User since 1990


    --
    Rod Giles
    Technical Director
    Elite Consulting Ltd.
    www.elite-consulting.com

    > Several great suggestions were mentioned (summarized below) but this
    > simple
    > problem is wupping us. Neither the Stiff Spring method of Enforced
    > Displacement or the Base Excitation method are returning expected results.
    > Either we are expecting the wrong thing, doing it all wrong, or Mechanica
    > is
    > broke and needs fixing.
    >
    > See this webpage for a description of the problem with screen shots.
    > http://www.solidpe.com/BaseExcitation.htm
    >
    > First, using the Stiff Spring method recommended by Mr. Holst we were
    > getting enforced displacements of 0.0025 inches with 125 lbf acting at a
    > 1000 lb/in spring...way short of the 1/8" that that force should have
    > produced. Besides, the harmonic (16.xx Hz) of the ruler itself was
    > showing
    > up in the (spring mounted) base even though the spring is way stiffer than
    > the ruler.
    >
    > Second, the Base excitation is returning screwy Base Displacements (see
    > webpage above).
    >
    Terms & ConditionsAccessibility statement