Harmonic analysis

Use the Harmonic-Full Method and Harmonic-Mode Superposition solution types to determine the steady-state response of a linear structure to loads that vary sinusoidally (harmonically) with time. In a harmonic analysis, the software calculates the structure's response at several frequencies. You can use harmonic analysis to verify whether a design can sustain the effects of forced vibrations, such as resonance and fatigue.

Loads for a harmonic analysis

When you apply a load for a harmonic analysis, you must typically specify the following properties for the load:

• Amplitude, which is the maximum value of the load, such as force or pressure. You define the amplitude value when you create the load.

• Forcing frequency, which is the frequency range of the harmonic load. In Pre/Post, you use the options on the Harmonic Options tab in the Solution dialog box to specify the frequency range for the solution. These options correspond to the ANSYS HARFRQ command. You can also create a Frequency Table modeling object to define the forcing frequencies as an array.

• Phase angle, which is a measure of time by which the load either lags or leads a frame of reference. In Pre/Post, you use the Phase Angle option in the Solution Step dialog box to define the phase angle. ANSYS applies a unique phase angle to all loads and constraints in the current solution step. To change the phase angle, create a new solution step.Note: Pre/Post applies any loads as the real component of the complex axis plane. The load and the phase angle must be consistent.

Modal steps precede harmonic steps in Harmonic Mode Superposition solutions

Your solution must include a Modal Loads step immediately before the appropriate type of harmonic step. ANSYS extracts mode shapes during the Modal Loads step and then uses them to calculate the harmonic response.

Note:

Only forces, accelerations, and the load vector that you created in the Modal Loads step are valid in the harmonic step.

In the Solution dialog box, use the Scale Factor for Loads Created in Modal Step (LVSCALE) option on the Harmonic Options page to specify how to scale the load vector. During the harmonic step in the solution, ANSYS scales all loads that you applied during the Modal Loads step, including forces and accelerations.

Note:

When you export or solve the input file, regardless of how many steps you create in Pre/Post, this software writes out only two ANSYS steps to the input file: Step - Modal Loads and Harmonic Mode Superposition - Loads, Constraints. Pre/Post writes out all loads and constraints in the Step - Modal Loads step only. When you solve the solution, ANSYS propagates all loads and constraints in the Step - Modal Loads step to the Harmonic Mode Superposition - Loads, Constraints step, unless LVSCALE = 0. In Pre/Post, you can apply temperature and pressure loads in Step - Modal Loads step since the phase angle is not applicable, whereas forces, moments, accelerations and constraints may have different phase angles.

Where do I find it?

Application	Pre/Post
Prerequisite	A FEM file as the work part and displayed partANSYS as the specified solverStructural as the specified analysis typeHarmonic-Full Method or Harmonic-Mode Superposition as the specified solution type

Look up more details

Transient dynamic analysis

Thermal-structural multiphysics analysis

Nonlinear buckling analysis

Performing a nonlinear buckling analysis

Cyclic symmetry analysis in ANSYS

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Harmonic analysis, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });