Page 150 - Using ANSYS for Finite Element Analysis A Tutorial for Engineers

stAtIc AnAlysIs usIng AreA elements • 137
(Alternatively, the command line code for the preceding step is
ET,1,PLANE82 followed by KEYOPT,1,3,3.)
Under the Extra Element Output K5, select nodal stress.
4. Define the geometric contents:
Preprocessor > Real Constants > Add/Edit/Delete
Enter a thickness of 20 mm.
(Alternatively, the command line code for the preceding step is
R,1,20.)
5. Element material properties:
Preprocessor > Material Props > Material Library > Structural >
Linear > Elastic > Isotropic
We are going to give the properties of steel. Enter the following when
prompted:
EX 200000
PRXY 0.3
(The command line code for the preceding step is MP,EX,1,200000
followed by MP,PRXY,1,0.3.)
Mesh Size
Preprocessor > Meshing > Size Cntrls > Manual Size > Areas > All
Areas
Select an element edge length of 5. Again, we will need to make sure
the model has converged. (Alternatively, the command line code for the
preceding step is AESIZE,ALL,5.)
6. Mesh:
Preprocessor > Meshing > Mesh > Areas > Free
And, select the area when prompted.
(Alternatively, the command line code for the preceding step is
AMESH,ALL.)