Transient Stress

Transient stress analysis is used to analyze events with known time-varying loads, small displacement, and linear material models. With transient stress, you can produce the dynamic response of a structure subjected to time-varying loads. Add ground acceleration components in any or all three global directions to determine the dynamic response.

Two types of transient stress analysis can be performed. Transient Stress (Direct Integration) uses time step-by-step integration algorithms to solve the equations of motion. This method is better suited than modal superposition when shock-type loads are applied to the model. Transient Stress (Modal Superposition) combines the results of a modal analysis. The natural frequency (modal) analysis must include enough modes to cover the contribution of the applied loads. Both direct integration and modal superposition can be used for transient loads that are not shock-type loads. One advantage of modal superposition results if the same model must be analyzed with different transient loads. After the modal analysis is complete, several Transient Stress (Modal Superposition) analyses can be performed with a relatively small computational effort.

Note: Transient stress (modal superpositon) uses the results from a modal analysis and operating systems create files with different formats. So both the modal analysis and transient stress analysis must 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.)

For the Transient Stress (Direct Integration), build the model and apply the loads. The general steps in performing a Transient Stress (Modal Superposition) analysis are as follows:

Set up the model for a Natural Frequency (Modal) analysis or Natural Frequency (Modal) with Load Stiffening. The calculated mode shapes are combined during the transient stress analysis. 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 can dictate a different minimum.)
Run the natural frequency (modal) analysis.
While reviewing the natural frequency results, find the node numbers where the loads are desired. (This step can be skipped if the load is a ground motion load, in which case the load is automatically applied through the boundary conditions.)
Copy the model to a new design scenario. (Right-click the current design scenario heading in the tree view and select Copy.)
Change the analysis type of the new design scenario to transient stress (modal superposition). (Analysis Change Type Linear Transient Stress (Modal Superposition))
Enter the loads and parameters in the Analysis Parameters dialog box.
1. Indicate which design scenario has the modal results.
2. Specify the nodal loads.
3. Other types of loads applied to the model have no affect on the analysis.
Perform the analysis.
When the analysis is complete, review the results in the Results environment. Use the Results Options: Load Case menu to view the response at each time step. When using ground acceleration, keep in mind that the results are relative to the ground excitation.