Dynamic Design Analysis Method (DDAM)


Dynamic Design Analysis Method (DDAM) is a U.S. Navy standard procedure for shock design. Engineers can use DDAM to analyze the shock response at the mountings of shipboard equipment – such as masts, propulsion shafts, rudders, exhaust uptakes and other critical structures – due to underwater explosions. All mission-essential equipment on board surface ships and submarines must be qualified for shock loads, such as from depth charges, mines, missiles and torpedoes.

 

DDAM simulates the interaction between the shock-loaded component and its fixed structure. The free motion of a vessel in water will produce a higher shock spectrum than a heavy structure would on ground. DDAM takes this effect into account in relation to the weight of the equipment, mounting location and orientation of the equipment on the vessel.

 

After performing a natural frequency analysis to determine the mode shapes and natural frequencies, a DDAM analysis is performed using an input spectrum of shock design values (displacements or accelerations). The input spectrum values are provided automatically by the software, based on data from unclassified U.S. Navy documents (primarily Naval Research Laboratory Report NRL-1396). Optionally, the user can provide user-defined coefficients, which could be for an alternate unit system, or classified coefficients. The security of classified coefficients is maintained through the ability to run the DDAM portion of the analysis on a secured computer.

 

Note

The provided input spectrum is based on units of pound-force, inches, and seconds for force, length, and time. All analyses that use this input spectrum must be performed with these units. (The other units are not restricted.) The natural frequency analysis would need to be performed in this unit system as well.

 

The DDAM analysis processor uses the Naval Research Laboratory (NRL) summation method to combine the peak responses from all mode shapes into overall displacements and stresses. Results can be viewed for each mode shape and the resultant in the Results environment.

 

Note

Since DDAM uses the results from a modal analysis, and since operating systems create files with different formats, both the modal analysis and DDAM analysis need to be performed on the same operating system. (Technically, the "endian" determines the file format. Any combination of operating systems using the same endian can be used for both analyses.)

 

The general steps in performing a DDAM analysis are as follows:

  1. Set up the model for a Natural Frequency (Modal) analysis or Natural Frequency (Modal) with Load Stiffening. The calculated mode shapes will be combined during the DDAM analysis, so the number of frequencies calculated in the modal analysis should be sufficient to excite the model in the appropriate directions. (Generally, the cumulative mass in the excited directions should be above a certain percentage, such as 80% although design codes may dictate a different minimum.)

  2. Run the natural frequency (modal) analysis.

  3. Copy the model to a new design scenario. (Right-click on the current design scenario heading in the tree view and choose "Copy".)

  4. Change the analysis type of the new design scenario to DDAM. ("Analysis: Analysis Type: Linear: Dynamic Design Analysis Method (DDAM)")

  5. Enter the direction and parameters in the Analysis Parameters dialog ("Analysis: Parameters...").

    1. Indicate which design scenario has the modal results.

    2. Specify the coefficients and directions. The load is transmitted to the model through the appropriate boundary conditions. (Spectrum in the X direction is transmitted through any boundary conditions that have X translation fixed, and so on.)

    3. Other types of loads applied to the model have no affect on the analysis.

  6. Perform the analysis ("Analysis: Perform Analysis...").

  7. When the analysis is complete, review the results in the Results environment. Use the "Results Options: Resultant" menu to toggle between the resultant and the response to each natural frequency. Use the "Results Options: Load Case" menu to view the response at each natural frequency. Keep in mind that the displacement results are relative to the ground excitation (input spectrum).