How does specified thickness affect results in a plane stress analysis?
|
In ANSYS Release 10.0, the thickness affects the in-plane stiffness for plane stress elements. The element stiffness is the volume integral of the transpose of the B matrix multiplied by the D matrix multiplied by the B matrix. The B matrix relates the strains to the displacement. The D matrix is the material matrix. If the thickness is constant, it can be removed from the integral, so the element stiffness is the thickness multiplied by the area integral of the transpose of the B matrix multiplied by the D matrix multiplied by the B matrix. If you do not specify a thickness for a plane stress element, a unit thickness is assumed. Below is a small test case. The results for the plane stress condition with no thickness specified and the plane stress condition with a thickness of 1.0 specified are identical. The results for the plane stress condition with a thickness of 2.0 specified are one-half the results for the plane stress condition with a thickness of 1.0 specified. For the plane stress assumption to be valid, the variation in displacement through the thickness (UZ) must be minimal (assumed to be zero), and the out-of-plane stress (sigma Z) must be minimal (assumed to be zero). These requirements are valid for both the plane stress condition without a thickness specified and the plane stress condition with a thickness specified. /prep7 et,1,182,2,,0 et,2,182,2,,3 r,2,1 et,3,182,2,,3 r,3,2 mp,ex,1,1036 mp,prxy,1,.3 /prep7 rect,0,1,0,1 rect,1.1,2.1,0,1 rect,2.2,3.2,0,1 esize,.125 amesh,1 type,2 real,2 amesh,2 type,3 real,3 amesh,3 nsel,s,loc,y,-.01,.01 d,all,all,0 alls nsel,s,loc,x,-.01,.01 nsel,a,loc,x,1.09,1.11 nsel,a,loc,x,2.19,2.21 nsel,r,loc,y,.99,1.01 f,all,fx,1000 alls /solu solve /post1 /view,,1,1,1 plnsol,s,x |
||
|