General Mechanical

General Mechanical

Harmonic Response

    • vigneshkrish333
      Subscriber

      Hello Community!!


      I know that, this is going to be a lengthy question. But please bear with me and help me to solve my problem. If it is not possible to completely answer here, I will be very glad, if you can forward me to some other helpful resources like Text Book, Web page, Online forum etc.,I am expecting a positive reply from you. I am in the tip of my project completion. If you can help me out in this I will be very happy.


      I am working on s project, where I have to perform Vibration Analysis in the Air compressor Piping system. In this regard I have simulated the fluid (compressed air) flow simulation in FLUENT module. I have also imported the pressure load from FLUENT to HARMONIC RESPONSE module, through "External Data Transfer" Component.


      I know that the compressor  running speed is 1200 rpm, which gives me 20 Hz of excitation frequency. I also know that the STRUCTURAL RESONANCE will occur when the Mechanical Natural Frequency (MNF) of the pipe is matching with the excitation frequency. In my case I found the MNF using MODAL analysis. In order to find the vibration amplitude (Frequency Vs Amplitude Curve)which is my requirement, I am going for HARMONIC RESPONSE analysis. In this case I have certain doubts, They are,


      1.(Fluent (Pressure load) - -> External data --> Harmonic response (Amplitude Vs frequency curve)) Is my procedure right to obtain the Amplitude Vs Frequency Curve?  


      2.While doing so, in harmonic response module as shown in following figure's bottom "Imported Pressure" region, there is a term called "analysis frequency" what does it mean? How it will affect my result?



      3. What does this error (shown in figure) mean? How to solve that? it is shown in following figure,



      4. While working on this, I found some solution to solve the above error. It is mentioned that to change the solution method "mode superposition" to "full". What does these solution methods mean?


      5. What does the "Phase Angle" mean while obtaining Amplitude Vs Frequency curve, which is shown in figure below,


       


       


       


      Thank You.


      Regards, 


      Vignesh.

    • peteroznewman
      Subscriber

      Hello Vignesh,


      1) Please reply with details about the Fluent model. Was it Transient or Steady State? If it was Steady State, then there are no oscillating pressures that would be relevant to a Harmonic Response analysis. If Fluent was a Transient solution, those results are not useful for a Harmonic Response. The Fluent Transient pressure load would be useful to drive a Transient Structural model.


      2) All loads in a Harmonic Response are sinusoidally time-varying. You specify three items: Amplitude, Phase and Frequency for the load. I think the relevant load is a 20 Hz unbalanced fan/motor attached to the piping. You need to obtain the unbalanced force created by that mechanical system.


      3) There are two methods to compute a Harmonic Response: MSUP and Full.  MSUP uses a Modal analysis to decompose the problem to a much smaller model but that comes with limitations, such as the inability to apply both Frequency and Spatially varying loads.  You can do that in Full, but I don't think you have the correct load in the first place.


      4) In Workbench, if you link the Solution cell of a Modal analysis to the Setup cell of a Harmonic Response, you are doing MSUP.  If you don't have that link, you are doing Full.


      5) If you have only one load, then the phase angle is not relevant.  The ANSYS Help page in the Mechanical APDL section 4.4 (link below) has a good example of when phase angle is important in Figure 4.3


      https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v195/ans_str/Hlp_G_STR4_5.html


      Follow these instructions to use the link above on the Student license.

    • vigneshkrish333
      Subscriber

      Thank you for your quick reply sir..


      1) My problem is to solve the vibrations in the compressor piping system. In this regard, the pressure at the outlet of the compressor is in pulsating nature (Transient Analysis).This is because the compressor is a reciprocating machine and it produces pulsating pressure.The pressure pulsation can be seen in the image shown below,


      The applied load is defined as y=1378+(55*(sin(2*PI*20*t))). For this pulsating pressure Boundary Condition I have used a UDF as shown in below figure



      Here it can be noted that the applied frequency has the frequcncy of 20 Hz, because the compressor running speed is 1200 rpm.


      After solving the above problem in the ANSYS FLUENT module I am getting the following pressure and velocity contours.




       


      Now my doubt is why we can't import this pressure load obtained in FLUENT to HARMONIC RESPONSE sir?


      What should I do now, so that I can plot the bode plot??


      Expecting a reply from you..


      Thank You

    • peteroznewman
      Subscriber

      Are you saying you were solving Fluent with a Transient solution?


      What was the simulation time for the plots above?


      Please show plots for 25 ms earlier.

    • vigneshkrish333
      Subscriber

      1. Yes sir, We are solving a Transient Solution in FLUENT module.


      2. The above attached plot's simulation time is 0.3 s


      I have attached the "Run Calculation" steps images below,



      3. what do you mean "Please show plots for 25 ms earlier" sir? I can't understand this.


      Do you need the plot for 0.275 s? 


      Thank You. Expecting a reply from you.

    • peteroznewman
      Subscriber

      The period of the pulsating pressure is 50 ms.  When you simulate with a 10 ms time step, you are putting just 5 points on a single cycle of a sinusoidal curve. That is a very poor representation of the curve. The recommendation is a minimum of 20 points per cycle, therefore you would have a time step of 2.5 ms.


      How are you initializing the simulation?  You could run a Steady State simulation and converge on a flow at the average pressure of 1380 kPa. Are you doing this? Then from this steady state flow, begin the Transient simulation and introduce the pulsations.  How many seconds are you simulating?  If your end time in the Transient is 2.5 seconds, that is 1000 time steps. 


      The oscillating pressure goes from peak to valley in 25 ms therefore, the forces on the walls are going to be different at the maximum pressure compared with the minimum pressure. Make a plot at two different times, one when the pressure is maximum and another plot when the pressure is minimum.

Viewing 5 reply threads
  • You must be logged in to reply to this topic.