This tutorial was completed using ANSYS 7.0 This tutorial is intended to outline the steps required to create an axisymmetric model.
The model will be that of a closed tube made from steel. Point loads will be applied at the center of the top and bottom plate to make an analytical verification simple to calculate. A 3/4 cross section view of the tube is shown below.
As a warning, point loads will create discontinuities in the your model near the point of application. If you chose to use these types of loads in your own modelling, be very careful and be sure to understand the theory of how the FEA package is appling the load and the assumption it is making. In this case, we will only be concerned about the stress distribution far from the point of application, so the discontinuities will have a negligable effect.
finish /clear /title, Axisymmetric Tube /prep7 /triad,off ! Turns off origin triad marker rectng,0,20,0,5 ! Create 3 overlapping rectangles rectng,15,20,0,100 rectng,0,20,95,100 aadd,all ! Add the areas together et,1,plane2 ! Define element type keyopt,1,3,1 ! Turns on axisymmetry mp,ex,1,200000 ! Young's Modulus mp,prxy,1,0.3 ! Poisson's ratio esize,2 ! Mesh size amesh,all ! Mesh the area finish /solu antype,0 ! Static analysis lsel,s,loc,x,0 ! Select the lines at x=0 dl,all,,symm ! Symmetry constraints lsel,all ! Re-select all lines nsel,s,loc,y,50 ! Node select at y=50 d,all,uy,0 ! Constrain motion in y nsel,all ! Re-select all nodes fk,1,fy,-100 ! Apply point loads in center fk,12,fy,100 solve finish /post1 nsel,s,loc,y,45,55 ! Select nodes from y=45 to y=55 prnsol,s,comp ! List stresses on those nodes nsel,all ! Re-select all nodes /expand,27,axis,,,10 ! Expand the axisymmetric elements /view,1,1,2,3 ! Change the viewing angle /replot