How to apply initial stress using INISTATE?
In ANSYS Release 11.0, initial stress can be applied using the INISTATE command. The example below is a simple tensile bar. It is solved twice. The first solution has one load step. The free end is loaded with a 1000 psi pressure. The calculated stress is 1000 psi and the calculated maximum displacement is 1 inch. The second solution has two load steps. In the first load step, an initial stress of 1000 psi is applied using INISTATE. The calculated stress is zero, because the applied initial stress is an internal load. Its effect will not be reflected in the calculated element stresses, because those stresses are caused by the external loads. However, its effect will be reflected in the DOF solution. The calculated maximum displacement is 1 inch. The calculated displacements reflect the DOF solution necessary to resolve the specified internal load. In the second load step, the initial stress is retained and a 1000 psi external load is ramp applied over two substeps. The applied external load is 500 psi in the first substep and 1000 psi in the second substep. In the first substep, the calculated stress is 500 psi and the calculated maximum displacement is 0.5 inches (1 + 0.5 = 0.5). In the second substep, the calculated stress is 1000 psi and the calculated maximum displacement is zero (1 + 1 = 0). /prep7 et,1,182 mp,ex,1,10e3 mp,nuxy,1,.3 rect,0,10,0,1 esize,2 amesh,1 nsel,s,loc,x,0 d,all,ux,0 d,node(0,0,0),all,0 nsel,s,loc,x,10 sf,all,press,1000 alls /solu outres,all,all solve /post1 prnsol,dof presol,s,comp /solu time,1 sfdele,all,all inistate,define,,,,,1000 outres,all,all solve time,2 nsubst,2 nsel,s,loc,x,10 sf,all,press,1000 alls solve /post1 set,first prnsol,dof presol,s,comp set,next prnsol,dof presol,s,comp set,next prnsol,dof presol,s,comp 

