This tutorial was created using ANSYS 7.0 The purpose of this tutorial is to outline the steps required to do a simple modal analysis of the cantilever beam shown below.
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,2 ! Modal analysis MODOPT,SUBSP,5 ! Subspace, 5 modes EQSLV,FRONT ! Frontal solver MXPAND,5 ! Expand 5 modes DK,1,ALL ! Constrain keypoint one SOLVE FINISH /POST1 ! List solutions SET,LIST SET,FIRST PLDISP ! Display first mode shape ANMODE,10,0.5, ,0 ! Animate mode shape