! ANSYS Rel.6.0. /TITLE, Plane Stress tension of an elastic plate with a hole /PREP7 ! Due to the symmetry of the problem we consider a quarter of the plate A=5 ! length of the plate quarter B=2 ! width of the plate quarter R=0.25 ! radius of the hole H=0.1 ! thickness of the plate P=1e3 ! magnitude of tensile load(kG/cm^2) !1kG = 9.8 N/m^2 MP,EX,1,2e6 ! Young's moduus EX=2*10+6 (kG/cm^2) MP,NUXY,1,0.3 ! Poisson's ratio NUXY=0.3 ET,1,PLANE82 ! Eight-node finite element PLANE82 (plane stress) ! ****************************************************** ! For stress analysis of the plate we can also choose shell element SHELL63, in this case uncomment the following commands !ET,1,SHELL63 !R,1,H !P=P*H ! pressure for a length unit (kG/cm) ! ****************************************************** K,1,0,0 ! Keypoints of the plate boundary: point number and coordinates K,2,A,0 K,3,A,B K,4,0,B A,1,2,3,4 ! Define area 1 using four keypoints ! Command A defines an area by connecting keypoints (max 18 points). Keypoints must be input in a clockwise or counterclockwise order around the area. APLOT,1 ! Show area 1 PCIRC,R ! Define area 2 - a cirlce with radius R and center in (0,0) ASBA,1,2 ! Substract area 2 from area 1 APLOT,ALL ! Show resulting area 3 ! Define parameters for finite element mesh ! KESIZE Specifies the edge lengths of the elements nearest a keypoint KESIZE,ALL,B/4 KESIZE,5,R/6 ! set element edge length near keypoint 5 KESIZE,6,R/6 ! set element edge length near keypoint 6 AMESH,ALL ! mesh area all areas (area 3) FINISH /SOLU ANTYPE,STAT ! set analysis type: static NSEL,S,LOC,X,A ! select all nodes with coordinate X=A SF,ALL,PRES,-P ! for all selected nodes set surface load PRES = -P NSEL,ALL ! select all nodes DL,9,,SYMM ! symmetry condition on line 9 (all lines with Y=0) DL,10,,SYMM ! symmetry condition on line 10 (all lines with X=0) ! ******************************************************** ! For finite element with degrees of freedom UX, UY the previous symmetry conditions on lines 9 and 10 are equivalent to the following commands !NSEL,S,LOC,X,0 !Select all nodes with coordinate x=0 !D,ALL,UX,0 ! for all selected nodes set displacement ux=0 !NSEL,S,LOC,Y,0 !Select all nodes with coordinate y=0 !D,ALL,UY,0 ! for all selected nodes set displacement uy=0 !NSEL,ALL ! select all nodes ! ******************************************************** SOLVE ! Solve finite element system of equations FINISH