MET 425 - FEA Applications II

Prof. Dave Johnson, psuprofdj@psu.edu
Penn State - Erie, The Behrend College

HW-8C:  Modal and Harmonic Analysis

Concepts: Pre-stressed Modal Analysis Harmonic Analysis Mode Superposition Method "frequency" domain vs. "time" domain analysis

The geometry of the Tacoma Narrows Bridge model (created by ANSYS Inc.) is provided in the Angel Lessons, HW Folder: bridge_13.0.agdb.  The file can be opened in WB 13.0 Simulation (Geometry > From File)

Use SI units (N, m, kg, sec)

FIRST, perform a static structural analysis to create the pre-stressed structural information.

• Define the thickness of the bridge deck (surface body) at 0.106 m
• The four leg towers are fixed at the base (vertex)
• The ends of the bridge (see figure, below, 3 lines at each end labeled A - across the end, plus lines on the left and right sides) are constrained to vertical and transverse motion (y- and z-directions).  The x-direction is "free"
• At the four vertices above the ends of the bridge (see figure, below - labeled B), use a fixed condition on the suspension cable system.

• Include standard earth gravity in the -Z-direction
• Mesh settings: Sizing, Use Adv. Size Function, OFF
• Solve and examine the deformed shape of the structure

Second, add a Modal Analysis and link the Initial Condition Environment to the Static Structural model (i.e., on the schematic page, drag and drop a modal analysis object onto the static structural solution).

• Request: 10 modes to find
• Activate the calculation of stress and strain
• Solve, observe the mode shapes and pick a mode that looks like the twisting bridge deck failure that could cause the failure of the Tacoma Narrows Bridge (Report that frequency and mode shape plot)

Third, add a New Analysis > Harmonic Response (i.e., on the schematic page, drag and drop a harmonic analysis object onto the modal "Model."  We do NOT want to link up the modal "Solution" which included the gravity load).

• Define a frequency range which spans all 10 frequencies you found in the Pre-stressed Modal Analysis
• Use the (default) method, Mode Superposition, with 50 solution intervals, no clustering of results
• Add a 0.03 Constant Damping Ratio (3% of critical damping)
• Apply a Pressure Load to the bridge deck (surface), by Components, with Y value of 10100 Pa
• Copy and paste the structural constraints (Fixed and Displacement conditions, NOT the Std. Earth Gravity) to the Harmonic Response simulation.  Edit/correct any problems in the "pasted" constraints.
• Solve the Harmonic Analysis

Because these results are in the "frequency domain" (not in the "time domain"), looking at Harmonic Response has two options:

1. Graph response at a point vs. frequency
2. Graph model response at a specific frequency

Insert a Frequency Response > Deformation, scope to one of the vertical "suspenders" near, but not at the middle of the bridge; find the Maximum response in the Z-direction.

Insert a Total Deformation Result, scoped to All Bodies, at Frequency of 0.4 Hz and Phase Angle of 0.

Turn in:

• a plot showing the element mesh of this system.  Document the number of nodes, elements, and all element types.  Record the total weight of the model carried JUST by the towers (Static Structural > Reaction Probe on the fixed support of the four leg towers, Z-axis direction)
• a plot showing the environment (ALL loads and constraints for the Static Structural solution)
• a plot of the total deformation for the Static Structural solution
• a plot (or plots) of the mode shape(s) which show the twisting bridge deck failure mode you selected (Pre-stressed Modal Solution)
• a listing of the 10 natural frequencies determined in the Pre-stressed Modal Solution
• the frequency response graphs (amplitude and phase angle) for the Harmonic Response solution
• the total deformation plot at frequency of 0.4 Hz and phase angle of 0 for the Harmonic Response solution