This tutorial was created using ANSYS 7.0 The purpose of this tutorial is to explain the steps required to perform Harmonic analysis the cantilever beam shown below.
We will now conduct a harmonic forced response test by applying a cyclic load (harmonic) at the end of the beam. The frequency of the load will be varied from 1 - 100 Hz. The figure below depicts the beam with the application of the load.
ANSYS provides 3 methods for conducting a harmonic analysis. These 3 methods are the Full , Reduced and Modal Superposition methods.
This example demonstrates the Full method because it is simple and easy to use as compared to the other two methods. However, this method makes use of the full stiffness and mass matrices and thus is the slower and costlier option.
FINISH /CLEAR /TITLE, Dynamic Analysis /PREP7 K,1,0,0 ! Enter keypoints K,2,1,0 L,1,2 ! Create line ET,1,BEAM3 ! Element type R,1,0.0001,8.33e-10,0.01 ! Real Const: area,I,height MP,EX,1,2.068e11 ! Young's modulus MP,PRXY,1,0.33 ! Poisson's ratio MP,DENS,1,7830 ! Density LESIZE,ALL,,,10 ! Element size LMESH,1 ! Mesh line FINISH /SOLU ANTYPE,3 ! Harmonic analysis DK,1,ALL ! Constrain keypoint 1 FK,2,FY,100 ! Apply force HARFRQ,0,100, ! Frequency range NSUBST,100, ! Number of frequency steps KBC,1 ! Stepped loads SOLVE FINISH /POST26 NSOL,2,2,U,Y, UY_2 ! Get y-deflection data STORE,MERGE PRVAR,2 ! Print data PLVAR,2 ! Plot data