Regarding pile stub creation in SACS

Hi friends,

I would like to find natural frequency for a tower along with the linearised pile. (by creating a pile stub)

While creating pile stub, I would like to know why stiffness matrix is created only for lateral loads at pile head joint. In my case, while calculating natural frequency I don't have any lateral deflection/force at pile head joint. In this case, people in the forum kindly guide me how to proceed further. 

Also while assuming pile stub behavior, kindly explain on how this rigid link and elastic behavior is assumed.Thank you in advance. 

  • I would not use the pile stub option to do this type of analysis. Instead try creating a pile superelement using the Create Pilehead Super Element analysis. This analysis will convert the pile soil interaction input file (psiinp) into a linearized superelement which can then be used to determine your eigenvalue solutions and mode shapes. Follow this workflow to perform this analysis:

    1. Static - Create Pilehead Super Element
      1. Input
        1. SACS Model File (sacinp)
        2. PSI Input File (psiinp)
      2. Output
        1. Foundation Superelement File (dynsef)
    2. Dynamic - Extract Mode Shapes
      1. Input
        1. SACS Model File (sacinp)
        2. Foundation Superelement File (dynsef)
      2. Output
        1. Dynpac Modal Solution File (dynmod)
        2. Dynpac Mass File (dynmas)
        3. Output Listing File (dynlst)

    Make sure that you use an equivalent  static load that closely resembles the load experienced during the dynamic event in question because the stiffness of the soil (and in turn, the eigenvalue solution) is dependent upon the applied load. In spectral wave fatigue analyses, you want something like an operating wave load and in seismic analyses you want some acceleration that resembles the acceleration experienced during the seismic event.

    You can refer to the section 2.5 of the PSI manual for generating foundation superelements using PSI and section 2.5.1 of the Dynpac manual for more information about including superelements in a Dynpac analysis.

    Regards,

    Geoff

  • Unknown said:
    Make sure that you use an equivalent  static load that closely resembles the load experienced during the dynamic event in question because the stiffness of the soil (and in turn, the eigenvalue solution) is dependent upon the applied load.

    Dear Geoff, do you suggest this case only for the instances governed by Quasi Static Analysis ??? 

  • No, this is for dynamic analyses since we are performing a dynamic response analysis. I suppose my equivalent static load terminology might be misleading, it should really just be:

    Make sure that you use an static load that closely resembles the load experienced during the dynamic event in question because the stiffness of the soil (and in turn, the eigenvalue solution) is dependent upon the applied load.
  • Consider an instance wherein i have used a static load (semblance of load experienced during dynamic loading). I have obtained the natural time period of the a slender structure as 5 seconds & Wave time period being 10 seconds (Load Frequency << Natural Frequency) . In this case, since the response is governed by stiffness of structure., it is a quasi static case.

    Hence, should we calculate DAF & input in SACS as Factored Load Case for Wave Loading ?? You are suggesting that the initially stated equivalent load is different from this Factoring of Wave load. Is my notion correct ??

  • You want to use a static load to linearize the piles that will be similar to the dynamic load. The easiest way to check is typically through comparing base shears. If you find that the static wave load results in a significantly different base shear than the dynamic loading result, you can consider applying a dynamic amplification factor to make the base shears the same. At the end of the day you are just trying to model the piles with a stiffness that would be similar to what is experienced during the dynamic event.