This tutorial was completed using ANSYS 7.0. The purpose of this tutorial is to explain how to apply distributed loads and use element tables to extract data. Please note that this material was also covered in the 'Bicycle Space Frame' tutorial under 'Basic Tutorials'.
A distributed load of 1000 N/m (1 N/mm) will be applied to a solid steel beam with a rectangular cross section as shown in the figure below. The cross-section of the beam is 10mm x 10mm while the modulus of elasticity of the steel is 200GPa.
/title, Distributed Loading of a Beam /PREP7 K,1,0,0 ! Define the keypoints K,2,1000,0 L,1,2 ! Create the line ET,1,BEAM3 ! Beam3 element type R,1,100,833.333,10 ! Real constants - area,I,height MP,EX,1,200000 ! Young's Modulus MP,PRXY,1,0.33 ! Poisson's ratio ESIZE,100 ! Mesh size LMESH,ALL ! Mesh line FINISH /SOLU ANTYPE,0 ! Static analysis DK,1,UX,0,,,UY ! Pin keypoint 1 DK,2,UY,0 ! Roller on keypoint 2 SFBEAM,ALL,1,PRES,1 ! Apply distributed load SOLVE FINISH /POST1 PLDISP,2 ! Plot deformed shape ETABLE,SMAXI,NMISC, 1 ! Create data for element table ETABLE,SMAXJ,NMISC, 3 PLLS,SMAXI,SMAXJ,1,0 ! Plot ETABLE data