Can ANSYS solve this plate buckling problem accurately? The following explains a simple test of buckling analysis of a plate in ANSYS.
Plate parameters:
Size: b = 112.8 in, a = 720 in.
Thickness: h = 1 in
Young's Modulus: E = 29000 ksi
Poisson's Ratio: nu = 0.3
Yield strength: fy = 50 ksi
Boundary condition: simply supported (moment free)
Our equation for the buckling capacity with
a/b = 720/112.8 = 6.4, k=3.29, gives Fcr = 8.24 ksi.
|
The input below file is for the buckling solution for all edges simply supported. Using your equation the buckling stress is 8240psi or 8.24ksi. The ANSYS solution using the file is 8175psi, so that is pretty close agreement. /PREP7 BLC4,0,0,112.8,720 MP,EX,1,29e6 MP,PRXY,1,0.3 ET,1,SHELL281 R,1,1, , , , , , LESIZE,2, , ,73, , , , ,1 LESIZE,1, , ,9, , , , ,1 LESIZE,3, , ,9, , , , ,1 LESIZE,4, , ,73, , , , ,1 AMESH,1 FINISH /SOLU ANTYPE,STATIC PSTRES,ON DL,1, ,UY, DL,1, ,UX, DL,1, ,UZ, DL,3, ,UZ, DL,2, ,UZ, DL,4, ,UZ, SFL,3,PRES,1, SOLVE FINISH /SOLUTION ANTYPE,1 BUCOPT,SUBSP,1,0,0 SOLVE FINISH /POST1 SET,LIST |
||
|