Carnegie Mellon University Mechanical Engineering

Problem 1 : Plate with Uniform Load

Problem Description

# Material : The plate is made of steel with Modulus of elasticity E = 30,000 ksi, and Poisson's ratio = 0.3
# Unit : U.S. Customary Units ONLY. It is important to convert all forces to "lb" and all dimensions to "in".
# Boundary Conditions : The plate is constrained from displacement in the x and y direction at (x=0", y=1") and from displacement in the y direction at (x=4", y=1")
# Loading : Uniform tensile Load with magnitude 20,000 lb/in^2 acting on both left and right sides of the plate.
# Objectives :

1. To determine stresses, strains and displacements in the plate when the load is applied to the plate.
2. To model the plate with coarse mesh (4 element) and fine mesh (16 elements), and determine how the element resolution affects the stresses, strains and displacements.

# Things to hand in :

1. Query Stress xx
2. Query Strain xx
3. Query Strain yy
4. Query Displacement in x direction
5. Query Displacement in y direction
6. Plot Stress xx VS. y
7. Plot Stress yy VS. y
8. Plot Shear stress xy VS. y
9. Combine 6, 7, 8 in one plot

# Figure :

1. Specify Geometry

Click on the following in the drop down menu on your right.

PREPROCESSOR -> -Modeling - Create

      CREATE -> -Areas -Rectangle

            RECTANGLES -> By Dimensions...



The input box "CREATE RECTANGLE BY DIMENSIONS" should now appear on the screen. According to the problem description, we have to create a plate with dimensions of 4 inches long and 2 inch high. Enter the corresponding x and y coordinates in the box as shown in the figure below. This will create a rectangle of size 2 inches x 4 inches.

Note: Since this example can be modeled as a plane stress problem, it is easier to create the plate as a two dimensional area instead of a volume. If the thickness is not specified otherwise, ANSYS assumes 1 in. into the screen.



After finish entering all the values, click OK. (DO NOT click Apply and then OK. This will place two rectangles in that location!)

Now the blue rectangular plate should appear on your ANSYS GRAPHICS window.