**Response Spectrum Analysis**

**Introduction**

Response Spectrum Analysis (RSA) is a technique used to estimate the maximum response of a structure for a transient event.

The technique combines response spectra for a specified dynamic loading with results of a normal modes analysis.

Response spectra describes the maximum response versus natural frequency of a 1-DOF system for a specified dynamic loading. They are employed to calculate the maximum modal response for each structural mode. These modal maxima may then be combined using various methods, such as the Absolute Sum (ABS) method or the Complete Quadratic Combination (CQC) method, to obtain an estimate of the peak structural response.

RSA is a simple and computationally inexpensive method to provide an approximation of peak response, compared to conventional transient analysis. The major computational effort is to obtain enough normal modes to represent the entire frequency range of input excitation and resulting response. Response spectra are usually provided by design specifications; given these, peak responses under various dynamic excitations can be quickly calculated.

Typical usage of this method is:

- evaluation of structure/substructure responses to seismic excitations.
- evaluation of naval or submarine equipment responses to shockwaves (explosions).

**Spectrum calculation**

Typically, the spectrum curve comes from some industry standards or criterions. If data are not available spectrum curves need to be generated using transient analysis. This can be done with a half-sine function as the time history of the input acceleration. The load is applied to the structure and its response in terms of time history acceleration is calculated. Finally, the frequency spectrum curve is calculated from acceleration (Figure 1), using, for example, Hypergraph **srs** math function.

Figure 1: Spectrum response calculation

**Analysis Method – Phase 1**

** **

Any structure can be represented by a serial of 1DOF oscillators using mode superposition method. Each mode is a single DOF oscillator.

In Phase 1, the system designers do not know the subsystem in detail, so they use a serial of SDOF oscillators to represent the subsystem. They calculate the response of each SDOF oscillators and take the peak value of each response curve.

Then they rank these peak values in frequency domain to get the Spectrum Curve. This can be repeated for a different damping to get a serial of spectrum curves.

**Analysis Method – Phase 2**

The spectrum curve can be combined with mode shapes (f) and modal participation factors (MPF), which can be got by normal modes analysis.

where u is the value of spectrum curve for resonant frequency and specific damping. Because the resonant frequency of real subsystem will not match the specified frequency of SDOF oscillators, we would interpolate by frequency and damping using these spectrum curves.

As a summary, the spectrum method is a way to combine (ABS, SRSS, NRL, NRC, CQC etc.) the maximum response values of each mode, and do not take care of if the subsystem can get these peak values at the same time.

This means that the result of spectrum analysis will be larger than real response. (If we use the transient analysis for the assembly which includes the detail subsystem mesh and detail residual system mesh, we can get the real response.)

Another characteristic of spectrum is that the curve is not calculated by FFT, so we cannot convert a spectrum curve to time domain by IFFT.

**DDAM (Dynamic Design Analysis Method)**

DDAM is a design method for the evaluation of shock resistance of shipboard equipment which is essentially linear and elastic, and which does not rest upon noise or vibration mounts that are non-linear. In essence this method presented a simplified modal analysis method in which the values to be used in the design check are prescribed by means of design shock spectra which are functions of the modal weight(s) and frequency(s) of the equipment-and-foundation system. Details on the DDAM process can be found in USA Naval Research Lab Memo 1396 among other documents.

**DDAM with Hperworks**

**DDAM Pre/Post for Reponse Spectrum Analysis with Shock Spectra**

The Hyperworks DDAM utility is used to setup a DDAM analysis for Optistruct, Nastran or Abaqus.

From the Optistruct, Nastran or Abaqus User Profiles, the utility can be launched from Tools à DDAM:

The utility requires that a normal modes result is available for the model. Support for Optistruct *.out files, Abaqus *.dat files and Nastran *.f06 files is included. To select this file, click the browse icon, select the file and select “Import”:

By default, the utility automatically selects modes that have the largest contribution until the minimum cumulative model weight of 80% is achieved. These modes are highlighted in greyscale. By default, the GUI shows these modes for the contribution in the X-Direction:

You may change the mode selection with the radio buttons:

Where:

**Significant** – Automatically selects mode based on modal weight until a cumulative contribution is met.

**All** – Selects all modes. Not realistic for very large models and frequency ranges due to size of output files. Should be used on smaller output files.

**Manual** – Allows the user to manually select any selection of modes.

Some other options include:

**Minimum cumulative modal weight** – Target of percent model weight required for analysis.

**Percent Selected Modal Weight** – Summation of percent modal weight currently selected. This field will be green if greater than Minimum cumulative modal weight, yellow if close and red if more modes are needed.

**List mode** – Modes are listed in a sortable table. (Default) They can be selected manually in this view.

**Graph mode** – Modes are displayed in a bar chart:

Once the user has selected the modes of concern, the DDAM coefficients can be selected based on the following loading conditions (taken from the NREL 1396 document):

**Ship Type** – Submarine or Surface Ship

**Mounting System** – Hull, Deck or Shell Plating

**Deformation Type** – Elastic, Elastic-Plastic or Half-Elastic

If the user chooses to manually specify these coefficients, they may do so by selecting “Specify values” which enables the tabular input for all possible coefficients:

By default, the values are pre-populated with the NREL 1396 values.

Once satisfied with the selected modes, and coefficients, the user may then calculate the Shock Spectra Curves via the “Calculate Spectrum” button. This populates the mode table and weighted average Da values:

The user may also choose to view the Shock Spectra curves in the Results Tab:

Where:

**Plot Type –** *Acceleration vs. Frequency* (Line chart) – Available only after shock spectra calculation

*Frequency vs. Mode* (Bar Chart) - Available after importing deck

*Effective weight vs. Frequency* (Bar Chart) – Available after importing deck

**Shock Modes** – *Significant* (Available with the bar graphs: Frequency vs. Mode and Effective weight vs. Frequency)

*All*.

In order to export your shock spectra curves to HM, select “Export to HM”:

The Shock Spectra curves will then be added to the user’s Hypermesh database and can be used for subsequent Response Spectrum Analysis in either Optistruct, Nastran or Abaqus:

**DDAM Setup Tutorial for a Foundation Bracket**

- Open file
*Model DDAM_v1.hm*

- Create a load collector for a simple normal modes analysis using the EIGRL card.

- Create a load step for the normal modes analysis

- Create the PARAM inputs for

**COUPMASS****EFFMASS**

Turning on EFFMASS computes and outputs the modal participation factor, which measures how close each mode is to a rigid body mode. This also calculates the modal effective mass which measures how much mass is associated with each mode. This allows the DDAM script to determine which modes contribute the most to the modal weight.

- Run the normal modes analysis using Optistruct

- Once the normal modes analysis is complete, go back into HyperMesh and run the DDAM script.

- Load the .out generated by the normal modes analysis:

- Adjust the loading values to the appropriate scenario and press the “Calculate Spectrum” button. Then press “Create Loadsteps” to add the loadsteps to the model.

- Check to see if the correct loadsteps and collectors were added.

These added collectors are your shock spectrums in the x, y, and z direction.

- Create a Control Card for GLOBAL_OUTPUT_REQUEST and turn on STRESS.
- Set the format to H3D (HyperMesh output-more robust list of outputs) and set Type to ALL

- Run the updated model in Optistruct.
- View your results.