General Mechanical

General Mechanical

Modal Analysis of Model Floor

    • zchini
      Subscriber

      I've been trying to setup a modal analysis test for a floor I've already experimented on in real life. The test I did in real life found the natural frequency of the floor to be about 8.02 HZ, but every time I run a simulation in ANSYS, I can't get the natural frequency to be below 29 Hz. I did a frequency sweep of the floor from 1 Hz to 10 Hz via a shaker placed on top of the floor.

      I have attached my Solidworks files for the floor I'm working on, as well as a picture showing the model in ANSYS. The ANSYS model has point masses of 33.5 lbm at coordinates (22in,27.79in,6.834in) and (22in,27.79in,17.084in) to represent the shaker that was put on the floor to initiate vibrations. The 4 top and bottom sheets of the floor, labelled "al_floor_sheet", are AL 6061-T6, and every other part is structural steel.

      I have tried:
      -making the bottom of each of the legs fixed supports
      -making the each of the legs fixed cylindrical supports
      -making 2 of the legs displacement supports free in the vertical direction, the two others fixed
      -making 3 of the legs displacement supports free in vertical, other one fixed (this gave me my closest result to the real life experiment, but I don't know if it makes sense)
      -many, many others

      I don't believe it is an issue with the dimensions of the floor, as I have double-checked them by reading the parts order forms and by measuring them myself, so the only thing I can think is wrong is how I'm setting up the experiment. Any insight would be greatly appreciated.

    • peteroznewman
      Subscriber

      Hello zchini,


      I expect that the vertical spacers are bonded to the top and bottom plates in your ANSYS model. I attach the SolidWorks view of the geometry.



      In the physical table, how are the vertical ribs connected to the top and bottom plates?  Is it just by the contact force generated by the bolts that go through the plates?



      If the contact between the top and bottom plates is only due to the pressure applied at the bolt, then there is a large area of the top and bottom plates that have no contact force with the vertical ribs. That means the top and bottom sheets are free to slide relative to the vertical ribs in the physical table, which results in low stiffness and a low natural frequency.


      If the model has completely bonded contact over the entire area, that results in a high stiffness and a higher natural frequency.


      If you attach an archive of your ANSYS model, I will have more information to advise you.


       

    • zchini
      Subscriber

      Thanks for the suggestion.


      My university was actually lucky enough to have some engineers from DRD come out to give a lecture of ANSYS for mechanical and CFD. They were kind enough to help me find out how to fix the floor simulation. You were right about the contacts between parts being the main issue, due to the upper and lower plates being attached to the internal structure via bolts. 


      To fix the issue, I started with a static structural simulation and applied forces to the tops and bottoms of the bolts, with the direction of the force pointing towards the floor. I tried to do a bolt pretension at first, but it was giving me issues, so I went with individual forces instead. I also changed the connections between the supporting plates in the floor and the surface plates on the top and bottom to frictional, with a coefficient of friction of .61, which is the coefficient I found for aluminum on steel. I then had the simulation run into a modal, and got the result I had been looking for.

    • peteroznewman
      Subscriber

      Modal Analysis is a linear analysis. That means a non-linear element like a frictional contact in the Static Structural model which can be open, slide or stick depending on the contact force and coefficient of friction, becomes a simple bonded contact if the contact is closed and no contact if the contact is open.

Viewing 3 reply threads
  • You must be logged in to reply to this topic.