General Mechanical

General Mechanical

MODAL ANAYLSIS: Should I use pre-stress or not?

    • Rameez_ul_Haq
      Subscriber
      Hello there. I am just starting on the modal analysis in order to extract the natrual frequencies of my structure. Under the Modal tree, I see a pre-stress option. Can anyone tell me should I use it or not? I read somewhere that if you are linking the static structural already solved system to your modal analysis, then the pre-stress will automatically come in your modal analysis. But I want to know why would I do that, rather than keeping the pre-stress option to 'none'?nCorrect me if I am wrong, does it mean that if I am having a forced vibration (i.e. an external force is being applied on the structure), then i should use the pre-stress, and if I don't have any force acting on my structure, then I shouldn't use the pre-stress? nIf I am using the forced vibration, i.e. with the pre-stress, will the modal analysis return me exitation frequencies or natural frequencies of the structure?nWhy do we need to add point mass to the structure in the modal analysis, if it is there?nHow can I check if the natural frequency of my structure is equal to the exitation frequency of it when load it applied on it, i.e. if resonance is occurring or not?n
    • Rameez_ul_Haq
      Subscriber
      Array, have already been so much grateful to you so helping me out and the other engineers out there. Thumbs up for your effort.nIf you can also kindly share your views on this one, would be really helpful n
    • peteroznewman
      Subscriber
      nMost structures that support machinery don't need a Static Structural model to pre-stress the structure prior to Modal analysis or a Harmonic Response.nStructures that require a Static Structural analysis to pre-stress the Modal generally have thin sections that are under high amounts of tension, for example a guitar string or the membrane of a drum head. The guitar string or drum membrane has an almost zero natural frequency when there is no tension on the structure. Once you apply the right amount of tension, you can raise that first natural frequency to the right note such as 110 Hz.nModal analysis has no loads, only mass, stiffness and supports. A machine has many parts, some of those are structural, meaning they carry load, while many other parts don't carry load such as wires, thermal or sound insulation and flimsy covers. Those parts add what is called non-structural mass (NSM). The NSM must be included in the model, but generally, those parts are deleted and only the structural parts are brought in to be meshed. ANSYS provides a way to smear that NSM over the entire structure using Distributed Mass. A few parts of the machine are concentrated massive component, such as an electric motor, or transformer. These parts are small compared with the whole structure and usually quite stiff from their own casing and bolt onto the main structure using a few bolts in a small pattern. Rather than mesh the motor casing, a Point Mass can be placed at the center of mass of the motor and a spider of elements reach back to the location of the few bolt holes that connect it to the structure. A correct Modal analysis should have the total mass equal to the actual mass of the fully assembled machine. If you don't put in all the mass, the natural frequencies will be higher than the frequencies experimentally measured on the structure.nOnce the Modal analysis has run, the resonant frequencies are known, but the amount of displacement in the Modal analysis is arbitrary because there was no load used in the analysis. To find out how much displacement will actually occur, a Harmonic Response analysis is dropped on the Solution cell of the Modal analysis. When a load is added to the Harmonic Response analysis, that is a periodic load and the magnitude is specified on the load item in the model, but the excitation frequency of that load is defined in the Analysis Settings. Typically a range of frequencies are specified and the solution tells you how much displacement magnitude every point in the model has for each excitation frequency in the analysis. The displacement is a magnitude of a periodic result that oscillates at the excitation frequency in the positive and negative directions. Obviously, the largest displacement magnitude occurs near the natural frequencies found in the Modal analysis.n
    • Rameez_ul_Haq
      Subscriber
      Array, If you don't put in all the mass, the natural frequencies will be higher than the frequencies experimentally measured on the structure, so basically if I have some parts within my structure, like motors or transformers as you said, which won't carry any load since the load will be carried by the main structure (which is actually holding these motors or transformers like under high accelerations) but you said that still these masses must be modelled as point/distributed masses while conducting the modal analysis. But I am trying to find out the natural frequencies of my main load carrying structure; still is it necessary for me to input these masses in my model while conducting modal analysis?nIn the second paragraph of yours, Typically a range of frequencies are specified and the solution tells you how much displacement magnitude every point in the model has for each excitation frequency in the analysis., So basically the displacement of each and every point within my model is dependent on two parameters: i) the excitation frequency at which the structure is forced to vibrate at ii) The magnitude of the periodic load. Can I also see the stresses within my Harmonic analysis, to see if the structure is failing or not under the specified load and excitation frequency?nAnd, this is kind of like a general question, should I expect failure within my main load carrying structure to occur if the excitation freq is not the same or near the natrual freq of it, but the amplitude of the load applied is very high which may cause some significant deformations within the structure, eventually leading it to fail? And also vice versa, meaning that can it be possible for the structure to not fail if the excitation freq is the same or near to the natural freq, but the amplitude of the load applied is not big enough to cause any plastic failure or fracture?nWill the response to my applied periodic load differ if I change the location at which the load is applied on my structure?nI must also confess that I got a little bit confused because if you think of a bridge which has a specific natural frequency, then I can vary the excitation frequencies in a range. But if wind is causing the excitation, then how will I get the load that should be inputted into the Harmonic response?nAnd one more thing, can you also kindly tell me the use of 'participation factor', 'effective mass', and 'ratio of effective mass to total mass'?n
    • peteroznewman
      Subscriber
      nI am trying to find out the natural frequencies of my main load carrying structure; still is it necessary for me to input these masses in my model while conducting modal analysis?nTo simulate the same frequency in Modal that the fully built machine will vibrate with after a hammer strike, you need all the mass that is hanging from that structure.nCan I also see the stresses within my Harmonic analysis, to see if the structure is failing or not?nHarmonic Response results are highly dependent on damping that is used in the model. If you underestimate the damping, the displacements and stresses will be overpredicted. There are ways to experimentally measure the damping of the structure to know that the model has a good value for damping. However, damping can be frequency dependent, so the first mode might have one value of damping while the 6th mode will have a different value of damping. As mentioned, the largest response is at the excitation frequency that matches the resonant frequency. Most machines with harmonic loads such as machines with high speed rotating parts are operated at a frequency away from any resonant frequency of the structure specifically to avoid a large harmonic response.nHowever, machines with high speed rotating parts often have to pass through a low resonant frequency on the way to the operating frequency. This is a Transient problem and the idea is that the system spends so little time when the excitation frequency matches the resonant frequency that there is no time for a large response to develop before the excitation frequency has passed by the resonant frequency.nthe amplitude of the load applied is very high which may cause some significant deformations within the structure, eventually leading it to failnKeep in mind that Modal analysis, Harmonic Response, Random Vibration and Response Spectrum analyses are all linear analysis methods. That means no nonlinear materials such as Plasticity, no large deflection, and no nonlinear contact can be included in the model. Linear analysis is most often used for performance analysis, and less often for evaluating failure. A full Transient Structural analysis, without any MSUP Modal analysis feeding in, can be used to include all nonlinear effects and can be used to evaluate failure conditions.nWill the response to my applied periodic load differ if I change the location at which the load is applied on my structure?nYes.ncan it be possible for the structure to not fail if the excitation freq is the same or near to the natural freqnEither the amplitude of the load is very small or the damping is very high.nBut if wind is causing the excitation, then how will I get the load that should be inputted into the Harmonic response?nA transient Fluid-Structure Interaction (FSI) analysis can predict the response of a structure to airflow.nhttps://medium.com/curiosityftw/busting-the-misconceptions-of-tacoma-narrows-bridge-collapse-467f830f9cc8nThe use of 'participation factor', 'effective mass', and 'ratio of effective mass to total mass' becomes relevant when deciding how many modes are required to have an accurate Modal Superposition (MSUP) method of calculating the Transient Structural, Response Spectrum or Harmonic Response analyses. n
    • Rameez_ul_Haq
      Subscriber
      thanks for the detailed overview.nWell, assume I have a load carrying structure, and there are some motors or other concentrated masses attached to the structure at some locations. Now, as you have also pointed out, I need to model these parts as point/distributed masses and the natural frequency of my load carrying structure will depend on the values and locations of these masses since they are the part of the overall structure. Now, if the motor is running at a specific freq (i.e. it is vibrating) and since it is interconnected to my main load carrying structure, it will excite it and make the overall structure to vibrate. If I already know the frequency at which the motor is running, then I just need to compare this freq if it is lying on any of the natural freq already determined using modal analysis of the overall structure. My question is how should I get the periodic load to enter to the harmonic response if I want to know the displacements within my load carrying structure?nShould I use 'Random Vibrations' for it? What are random vibrations and when should they be used?n
    • Erik Kostson
      Ansys Employee
      Good morning We have some very good courses which are free on the topics of Dynamic analysis (Modal and Harmonic say)nModal Analysis | Ansys Innovation CoursesnMode Superposition Method | Ansys Innovation CoursesnHarmonic Analysis of Structures - ANSYS Innovation CoursesnnAs for wind induced vibrations (assuming small vibrations so linear analysis), one could run a transient cfd/fluent analysis in fluent, then fast Fourier transform (FFT) the pressure fluctuations (done inside fleunt) on the structural surface and then impose those loads in a Harmonic analysis (we can import .cgns files from fluent that contain the fft of the pressure fluctuations).nnIf the vibrations are very high then we need a full 2 way transient analysis.nnAll the bestnErikn
    • Rameez_ul_Haq
      Subscriber
      Array, thank you n
    • peteroznewman
      Subscriber
      nMy question is how should I get the periodic load to enter to the harmonic response if I want to know the displacements within my load carrying structure?nApply the load at the location where it originates as an amplitude and direction in a Harmonic Response analysis. Make sure the damping has been properly defined. For a global propery, you can use Damping Controls under Analysis settings, The damping can be defined in Engineering Data if multiple materials are used in the structure. Don't do both because they are additive! Finally, in Analysis Settings, you must define a range of frequencies to analyze. This is the excitation frequency of the load. I recall that it didn't like being given a single frequency for the range. The software was written because most analysts want results over a range of excitation frequencies. If your target value was 330 Hz, just use 330 and 331 Hz for example.n
    • Rameez_ul_Haq
      Subscriber
      thank you for your answer. I will also have a look at the free courses on ANSYS to help me understand in depth the modal analysis, harmonic response and random vibrations.nJust one more question, if you may. For example I conduct a modal analysis and I see a range of natural freq for it. Now, one of the natural freq found out is equal/lower than the expected excited freq to occur on this structure in reality, in the same mode and same direction as of that natural freq.. In order to lest any possible resonance happening the reality, I want the structure to have the natural freq in that mode to be bigger than my excited freq. How can I achieve this? I mean I know this that increasing the stiffness of the structure will definitely soar the nautral frequencies up, but how and where should I stiffen up my structure so that under the same load/mode, the natural frequency increases (and having very less effect on the rest of the modes of natural freq)? nI can also decrease the mass at the same time to raise the natural freq, but I don't know how and where to decrease the mass to increase the natural freq of my structure in a specific mode? [Moreover, decreasing the mass corresponds to decreasing the stiffness of the structure as well, so essentially a paradox here].n
    • peteroznewman
      Subscriber
      nGreat question. I myself recently learned how to increase the natural frequency of a structure in a somewhat optimal way. nYou ask how to increase the natural frequency of the structure to move it above a known excitation frequency. I will get to that, but you should also consider the other approach, which is to decrease the natural frequency to a value well below the excitation frequency. Adding mass and reducing stiffness will accomplish that. This works well for machines that are on the ground, where the added weight is relatively unimportant. However, for machines that are airborne, or have to be lifted into space, those machines have strict weight limits, so adding mass is a highly undesirable solution. You also have to look at the next mode that may now be closer to the excitation frequency. This is where the mass participation comes in. If the excitation frequency is in the X direction, but the second mode has low participation in the X direction but high in the Y or Z directions, then there will be less concern. There is also the issue of transients when the excitation is sweeping up to its operating point and has to pass through the low natural frequency.nElement Strain Energy (ESE) is the metric used to quantify regions that contribute to the modal frequency. Create a User Defined Result and enter ENERGYPOTENTIAL for the expression to get a plot of continuum element strain energy. You need to turn on energy and stress as outputs in output control before you solve.nRegions of high element strain energy are not stiff enough. Regions of low element strain energy are stiffer and heavier than they need to be. An optimal way to raise the natural frequency is to reduce mass (and stiffness) in the areas of low ESE and increase stiffness (and mass) in the areas of high ESE. nThat being said, there are better and worse ways to increase stiffness. If you have a flat plate, one way to increase stiffness is to increase the thickness. That is is the worst way. A better way is to add a rib to the flat plate. The rib adds a lot of stiffness and very little mass. One example is a simple cantilever beam. If the initial design is a flat strip, the elements with high ESE will be at the base of the beam and the elements with low ESE will be at the tip of the beam. You could change the beam from a constant thickness to a tapered thickness. The base will be thicker than the tip. Now the ESE will be closer to equal at each end. If you raise a rib on the beam, that will more dramatically increase the natural frequency. If the rib is a constant height, the ESE will be higher on the rib at the base of the cantilever and lower on the rib at the tip. Again, the rib can be tapered and be taller at the base and shorter at the tip.nComponent Percentage of Total Strain Energy A machine may have tens or more than 100 structural parts. You don't want to look at the ESE on 100 parts because you don't want to redesign 100 parts. What you want to do is calculate the Total ESE on each part and sum that up for the machine, then calculate the percentage of the total for each part. Sort that list from high to low and now you know the most important part to redesign, and the relative importance of the second and third parts on that list.nThe issue with a FE model of a whole machine is if it has springs and/or joints with stiffness values included. The strain energy stored in those springs are not included in the ENERGYPOTENTIAL result, which only applies to continuum elements. Below is an excellent article that provides APDL code that can help to extract the strain energy out of these springs and sum the ESE in each component so that the sum of the ESE for the whole machine can be accurately calculated.nhttps://medium.com/swlh/energize-your-ansys-dynamic-mechanical-analyses-b94c58da9a30n
    • Rameez_ul_Haq
      Subscriber
      Array, well thanks for the long and comprehensive answer.nIf the excitation frequency is in the X direction, .... , if the excitation freq is the the same as one of the natural frequncies seen in after the modal analysis, but not in the same direction as i am seeing in the participation factor, so I shouldn't be concerned about any possible resonance occurring, right?n
    • peteroznewman
      Subscriber
      nRight. That is what the Harmonic Response does, it uses the Modal information, which includes the effective mass participation factor in each direction for each mode, and excites those modes according to that factor and the direction of the excitation.n
    • Rameez_ul_Haq
      Subscriber
      ,right now I just read the previous long explanation you made on how to modify the structure in order to alter its natural frequency.nWhile using the 'ENERGYPOTENTIAL', shouldn't I create an 'ENERGYPOTENTIAL' for all the modes which I feel are dangerous? I mean that assume I have 4 modes which I feel should be changed for my structure, so for each mode I should see where the ESE stored is higher and where is lower.nBasically, what you said is we need to increase the stiffness in those regions of a structure where the ESE is high since they are expected to relatively deform more than the rest of the structure. Moreover, we might also need to decrease the mass in the regions which has very less ESE since that redundant mass will (although increase the overall natrual freq values) is over-weighing the structure and might be of no use.nNow, if I try to increase the stiffness of my structure in those regions where the stiffness is low (or in other words, ESE is high), this means either I would increase the thickness of it or I would insert a stiffener, maybe a flange or a rib. But my question is won't it locally increase the mass there as well? I mean the stiffness and mass has an inverse relation when trying to alter the natural freq of that structure. Similarly, if I try to decrease the mass in the regions which are over-weighed, this would indirectly mean that I am decreasing the stiffness there as well, so I might not be getting the expected decrease in the natural freq.nFurthermore, what if I try to add the stiffeners to another location, i.e. to the low ESE locations instead of high ESE locations. Will it cause my natural freq [in a specific mode which I am trying to omit or get rid of) of my structure to increase as well? Maybe it will, but the increase in the natural freq of my structure in a specific mode might not be as much as if I add stiffener in the locations of the high ESE elements.n
    • peteroznewman
      Subscriber
      nYes, you can create an ENERGYPOTENTIAL result for each mode of concern. The first mode is generally the one of most concern because it generally has the largest response.nNatural Frequency = sqrt( K/M ) and adding or removing material affects both K and M at the same time, but think about the simple cantilever beam of uniform thickness. The material at the base of the cantilever has low mass participation in mode 1 compared to the material at the tip of the beam so adding mass at the base has a small impact on frequency. On the other hand, adding stiffness to the base of the cantilever has a large effect on the frequency. The opposite can be said about material at the tip of the cantilever.n
    • Rameez_ul_Haq
      Subscriber
      Array, well thank you n
Viewing 15 reply threads
  • You must be logged in to reply to this topic.