Pre-Analysis & Start Up

Analytical vs. Numerical Approaches

We can either assume the geometry as an infinite plate and solve the problem analytically, or approximate the geometry as a collection of "finite elements", and solve the problem numerically. The following flow chart compares the two approaches.

Let's first review the analytical results for the infinite plate. We'll then use these results to check the numerical solution from ANSYS.

Analytical Results

Displacement

Let's estimate the expected displacement of the right edge relative to the center of the hole. We can get a reasonable estimate by neglecting the hole and approximating the entire plate as being in uniaxial tension. Dividing the applied tensile stress by the Young's modulus gives the uniform strain in the x direction.

Multiplying this by the half-width (5 in) gives the expected displacement of the right edge as ~ 0.1724 in. We'll check this against ANSYS AIM.

Sigma-r

Let's consider the expected trends for Sigma-r, the radial stress, in the vicinity of the hole and far from the hole. The analytical solution for Sigma-r in an infinite plate is:

where a is the hole radius and Sigma-o is the applied uniform stress (denoted P in the problem specification). At the hole (r=a), this reduces to

This result can be understood by looking at a vanishingly small element at the hole as shown schematically below.

We see that Sigma-r at the hole is the normal stress at the hole. Since the hole is a free surface, this has to be zero.

For r>>a,

Far from the hole, Sigma-r is a function of theta only. At theta = 0, Sigma-r ~ Sigma-o. This makes sense since r is aligned with x when theta = 0. At theta = 90 deg., Sigma-r ~ 0 which also makes sense since r is now aligned with y. We'll check these trends in the ANSYS AIM results.

Sigma-theta

Let's next consider the expected trends for Sigma-theta, the circumferential stress, in the vicinity of the hole and far from the hole. The analytical solution for Sigma-theta in an infinite plate is:

At r = a, this reduces to

At theta = 90 deg., Sigma-theta = 3*Sigma-o for an infinite plate. This leads to a stress concentration factor of 3 for an infinite plate.

For r>>a,

At theta = 0 and theta = 90 deg., we get

Far from the hole, Sigma-theta is a function of theta only but its variation is the opposite of Sigma-r (which is not surprising since r and theta are orthogonal coordinates; when r is aligned with x, theta is aligned with y and vice-versa). As one goes around the hole from theta = 0 to theta = 90 deg., Sigma-theta increases from 0 to Sigma-o. More trends to check in the ANSYS results!

Tau-r-theta

The analytical solution for the shear stress Tau-r-theta in an infinite plate is:

At r=a,

By looking at a vanishingly small element at the hole, we see that Tau-r-theta is the shear stress on a stress surface, so it has to be zero.

For r>>a,

We can deduce that, far from the hole, Tau-r-theta = 0 both at theta = 0 and theta = 90 deg. Even more trends to check in ANSYS!

Sigma-x

First, let's begin by finding the average stress, the nominal area stress, and the maximum stress with a concentration factor.

The concentration factor for an infinite plate with a hole is K = 3. The maximum stress for an infinite plate with a hole is

Although there is no analytical solution for a finite plate with a hole, there is empirical data available to find a concentration factor. Using a Concentration Factor Chart (Cornell 3250 Students: See Figure 4.22 on page 158 in Deformable Bodies and Their Material Behavior), we find that d/w = 1 and thus K ~ 2:73 Now we can find the maximum stress using the nominal stress and the concentration factor

Start-Up

Now that we have the pre-calculations, we are ready begin simulating in ANSYS AIM. Open ANSYS AIM by going to Start > All Apps > ANSYS 18.1 > ANSYS AIM 18.1. Once you are at the start page of AIM select the Structural template in the top left corner as shown below.

You will be prompted by the Structural Template to either Define new geometry, Import geometry file, or connect to active CAD session. Select define new geometry and press Next. For this problem we will be using static calculation type. The Model Editor will launch automatically.

 
Go to Step 2: Geometry

Go to all (ANSYS or FLUENT) Learning Modules