Fast Nonlinear Analysis (FNA) is a modal analysis method useful for the static or dynamic evaluation of linear or nonlinear structural systems. Because of its computationally condensed formulation, FNA is well-suited for time-history analysis, and often recommended over direct-integration applications. During dynamic-nonlinear FNA application, analytical models should:

Be primarily linear-elastic.

Have a limited number of predefined nonlinear members.

Lump nonlinear behavior within link objects.

In addition to nonlinear material force-deformation relationships, these link objects may simulate concentrated damping devices, isolators, and other energy-dissipating technologies. If fuse mechanisms are not integral to the design intention, an initial elastic analysis may reveal locations where inelasticity is likely to occur. However, it is always best to predefine inelastic mechanisms such that their design may provide for sufficient ductility, while elastic systems are ensured sufficient strength. Capacity Design provides for a more reliable model and a better-performing structure.

The efficiency of FNA formulation is largely due to the separation of the nonlinear-object force vector R_NL(t) from the elastic stiffness matrix and the damped equations of motion, as seen in the fundamental equilibrium equation of FNA, expressed as:

Stiffness- and mass-orthogonal Load-Dependent Ritz Vectors condense the equilibrium relationships within the elastic structural system. At each time increment, the uncoupled modal equations are solved exactly, while forces within the predefined nonlinear DOF, indexed within R_NL(t), are resolved through an iterative process which converges to satisfy equilibrium. Following this procedure, FNA is an efficient and accurate dynamic-nonlinear application which satisfies equilibrium, force-deformation, and compatibility relationships.

FNA application process

Fast Nonlinear Analysis (FNA) may be implemented within SAP2000 using the process described in the FNA application process article.

Model. Create the analytical model.
Mass. Define the mass source through Define > Mass Source. Mass must be present within joint locations to enable formulation.
Modal load case. Modify the existing modal load case to use Ritz Vectors, which capture response more effectively when compared with the same number of Eigen Vectors, by selecting Define > Load Cases > Modal > Modify/Show Load Case > Ritz.
On the same form, under Loads Applied, select a Load Type and orientation which is suitable for the given model and investigation. For example, Accel and UX would be suitable for the lateral analysis of a 2D portal frame. Maximum Cycles and Participation Ratios may remain on default settings.

During analysis, data from the modal load case will then coordinate with the time-history load case.
Time function. Define the time function through Define > Functions > Time History. The existing ramp and uniform functions may be modified, or a function may be added from the various types available, including from the file of a time-history record.
Time-history load case. Add a new load case for the time-history analysis by selecting Define > Load Cases > Add New Load Case.
- Name the time-history load case.
- Select Load Case Type > Time History, Analysis Type > Nonlinear, Time-History Type > Modal.
- Under Loads Applied, select Load Type > Accel, Load Name > U1, then select the time function previously defined. If conversion from gravity units to distance units is necessary, enter the appropriate scale factor (32.2 converts to feet, 32.2*12 = 386.4 to inches).
- Enter an Output Time Step of ¹/₁₀ the fundamental period of vibration. A preliminary modal analysis may be run to compute this value. This time step will likely be more fine than the default value, and provide more detail in the output.
- Enter a quantity of time steps which coordinates the time-step size with the duration of loading.
Analysis. Run analysis with both the modal and time-history load cases.
Output. Various options are available for reviewing output, including:
- Graphically display member forces per time step by selecting Display > Show Forces/Stresses > Frames/Cables/Tendons. Next, specify the time-history load case, the time step, and the response quantity to review. Use the arrows at the bottom of the window to scroll through the range of dynamic response.
- The envelope of member forces may be displayed through a similar process where Envelope (Range) is selected under Multivalued Options.
- Deflection data and tabular output formats are also available.
- Animation. To create a video animation, have the desired type of response active in the current window, select File > Create Video > Create Multi-step Animation Video, then save the AVI file outside of the C:\Program Files\Computers and Structures\SAP2000 folder. The Multi-step Video File Creation form will then open. Enter animation details, including duration and magnification factor. Compress the video by selecting a compressor type and quality. Microsoft Video 1 at 75 should reduce the file size by approximately 25 times. The video will then be available in the specified location.
- Response spectrum. A response-spectrum curve may be plotted for a selected joint through Display > Show Response-Spectrum Curves. On the Axes tab, select the plot parameters, such as Period vs. PSA. Specify direction, damping, and any other pertinent options. Select Display, then the curve will generate for each damping level specified.
- Time-history traces. Time-history traces may be displayed for a selected joint through Display > Show Plot Functions. Select the joint from List of Functions, select Define Plot Functions, select the joint again, then select Modify/Show Plot Function. Select the response parameter from Vector Type, and the DOF from Component. Select OK > OK to leave these forms. Select the joint again, then select Add. Now that the Vertical Function is specified, select the Horizontal Plot Function, then save the Named Set if desired. Select Display to present the plot.