Project Report Structural Dynamics Harmonic response Fatigue (S–N)

Harmonic Response & Fatigue Life Assessment of a Bracket

Many components fail not because they exceed yield, but because repeated dynamic loading drives fatigue damage at stress levels well below static limits. This report summarizes a simulation workflow in ANSYS Mechanical to quantify modal behavior, resonance-driven amplification, and stress–life (S–N) fatigue life for a bracket subjected to harmonic excitation.

Technical summary • Modal + harmonic • Simulation-verified
Harmonic deformation of bracket at resonance

Harmonic response visualization used to identify resonance-driven amplification and critical deformation behavior.

Executive summary

  • Dominant resonance: ~158.5 Hz (primary amplification region)
  • Secondary resonance: ~380 Hz
  • Peak deformation (at resonance): ~8.6 mm (directional Z)
  • Peak alternating stress: ~202 MPa (equivalent von Mises)

Fatigue result (S–N)

  • Minimum predicted life: ~253 s at the critical hotspot
  • Method: Stress–Life (S–N), fully reversed (R = −1)
  • Domain: Time – Harmonic
  • Evaluation: single-frequency assessment at 158.52 Hz
Contents

Overview

Harmonic loading can produce response levels far above static expectations when the excitation aligns with a structure’s natural frequencies. In such cases, resonance-driven amplification elevates deformation and stress, often creating localized hotspots where fatigue cracks initiate. This workflow combines modal analysis, harmonic response, and stress–life fatigue to support design decisions early—before physical testing.

Why this matters: The same 10 kN load can be “safe” away from resonance but damaging near resonance. Identifying frequency-sensitive amplification regions is essential for robust durability design.

1) Model setup

The bracket is constrained at mounting locations using cylindrical supports. A 10,000 N harmonic force is applied at the free-end hole to represent periodic excitation during operation.

Boundary conditions using cylindrical supports
(a) Cylindrical supports at mounting holes.
Harmonic force application location
(b) 10,000 N harmonic force at free-end hole.

2) Mesh and harmonic analysis settings

A 3D solid mesh is used with refinement near geometric discontinuities (holes and cutouts) to resolve stress gradients. The harmonic response is solved using mode superposition over 0–500 Hz with linear spacing.

Mesh refinement near cutouts and holes
(a) Mesh with refinement near cutouts/holes.
Harmonic response settings for mode superposition
(b) Harmonic response settings (mode superposition, 0–500 Hz).

Modal analysis identifies natural frequencies and mode shapes that drive harmonic amplification. The frequency response indicates a dominant amplification region near ~158.5 Hz and a secondary region near ~380 Hz.

Mode 1 shape around 158.5 Hz
(a) Mode 1 shape (~158.5 Hz dominant).
Mode 2 shape around 380 Hz
(b) Mode 2 shape (~380 Hz secondary).
Extracted modal frequencies and participation
(a) Extracted modal frequencies/participation.
Frequency response showing resonance peaks
(b) Amplitude response showing resonance peaks.

4) Phase response

The phase plot shows a rapid transition across resonance (approximately π radians), which is a classic signature of a resonant system. This confirms the peak near ~158.5 Hz is resonance-driven rather than a static-like trend.

Phase angle versus frequency showing resonance phase shift

Phase angle vs. frequency — sharp phase change across resonance.

5) Harmonic stress and deformation at the critical frequency

At the dominant resonance (~158.5 Hz), dynamic amplification drives peak deformation and elevated alternating stress. Stress concentrations are localized near holes/cutouts—typical initiation sites for fatigue damage.

Directional deformation at resonance
(a) Directional deformation (Z) near resonance (~8.6 mm peak).
Equivalent alternating stress at resonance
(b) Equivalent alternating stress (~202 MPa peak).

6) Fatigue setup

Fatigue life is computed using the Stress–Life (S–N) method. The Fatigue Tool is configured in the Time – Harmonic domain using equivalent (von Mises) stress, evaluated at a single frequency (158.52 Hz) with an exposure duration of 600 s.

S-N curve for R = -1 fully reversed loading
(a) S–N curve (R = −1 fully reversed).
Fatigue tool settings in ANSYS Mechanical
(b) Fatigue Tool settings (Time–Harmonic, single frequency, 600 s exposure).

7) Fatigue life result

The fatigue life contour highlights the most critical hotspot under resonance conditions. The minimum predicted life is approximately 253 seconds, while non-critical regions show substantially longer life within the plotted range.

Fatigue life contour at resonance frequency

Fatigue life contour at the critical frequency (~158.5 Hz).

Design recommendations

Reduce resonance risk

  • Avoid excitation bands: if possible, shift operating conditions away from ~158.5 Hz and ~380 Hz.
  • Shift natural frequencies: increase stiffness (ribs/local thickening) or modify geometry to move the modes.
  • Add damping/isolation: damping treatments or compliant mounts can reduce amplification near resonance.

Reduce fatigue hotspot severity

  • Lower stress concentration: add fillets/smoother transitions near cutouts and holes.
  • Local reinforcement: increase section thickness near hotspots if packaging allows.
  • Verify fatigue inputs: validate S–N data and mean-stress/damping assumptions for final sign-off.

Need vibration and fatigue support?

We help teams identify resonance risks, quantify dynamic stress, and improve durability with simulation-backed design guidance. Contact us at info@tetraelements.com .

Schedule a free consultation Back to projects

Note: Results shown are from simulation of the presented configuration and analysis settings. Final hardware performance can vary with material properties, damping, boundary conditions, manufacturing tolerances, and real-world excitation profiles.