Page 155 - Using ANSYS for Finite Element Analysis A Tutorial for Engineers

142 • Using ansys for finite element analysis
Material Properties: Modulus of elasticity: E = 200GPa, Poisson’s
ratio: ν = 0.32
Geometry: Lengths and radii as shown, Thickness: 3 mm
Loading: Distributed load: 88 N/cm, Constraints: ux, uy, uz = 0 at
left hexagon

Solution Methodology
As the thickness (3 mm) is quite small compared to the overall length of
about 12 cm, the problem can be reasonably treated as a plane stress prob-
lem. In ANSYS, it will be treated as a plane stress with thickness problem.
The geometry will be created through rectangle, circle and hexagon
commands, together with Boolean operations of add (union) and subtract
(difference).
Step-by-Step ANSYS Solution

1. Start ANSYS:
File -> Save As -> Filename -> OK
2. Use the structural solid element PLANE82 for FEM modeling:
Preprocessor -> Element Type -> Add/Edit/Delete -> Add ->
Structural Mass-Solid -> Select 8node 82 -> OK -> Options -> Ele-
ment Behavior: Select Plane Stress w/thk -> OK -> Close
3. Enter real constants for the element type chosen:
Preprocessor -> Real Constants -> Add/Edit/Delete -> Add -> OK ->
Enter Thickness THK = 0.3 -> OK -> Close
4. Enter material property data for specified steel:
Preprocessor -> Material Props -> Material Model -> Structural ->
Linear -> Elastic -> Isotropic -> Enter Young’s modulus EX = 200e9
and Poisson’s ratio PRXY = 0.32 -> OK -> Close
Note: After each significant step, click SAVE_DB on ANSYS toolbar.