This tutorial was created using ANSYS 7.0 The purpose of this tutorial is to outline the steps required to do a simple nonlinear analysis of the beam shown below.
There are several causes for nonlinear behaviour such as Changing Status, Material Nonlinearities and Geometric Nonlinearities (change in response due to large deformations). This tutorial will deal specifically with Geometric Nonlinearities .
To solve this problem, the load will added incrementally. After each increment, the stiffness matrix will be adjusted before increasing the load.
The solution will be compared to the equivalent solution using a linear response.
/prep7 ! start preprocessor /title,NonLinear Analysis of Cantilever Beam k,1,0,0,0 ! define keypoints k,2,5,0,0 ! 5" beam (length) l,1,2 ! define line et,1,beam3 ! Beam r,1,0.03125,4.069e-5,0.125 ! area, izz, height of beam mp,ex,1,30.0e6 ! Young's Modulus mp,prxy,1,0.3 ! Poisson's ratio esize,0.1 ! element size of 0.1" lmesh,all ! mesh the line finish ! stop preprocessor /solu ! start solution phase antype,static ! static analysis nlgeom,on ! turn on non-linear geometry analysis autots,on ! auto time stepping nsubst,5,1000,1 ! Size of first substep=1/5 of the total load, max # substeps=1000, min # substeps=1 outres,all,all ! save results of all iterations dk,1,all ! constrain all DOF on ground fk,2,mz,-100 ! applied moment solve /post1 pldisp,1 ! display deformed mesh PRNSOL,U,X ! lists horizontal deflections