ANSYS WB - Plate With a Hole Demo - Results

Plate With a Hole Tutorial - Results

Geometry / Mesh

Before we look at the solution, lets look at the mesh. It is below.

The first thing to notice about the plate with the hole geometry is that the domain is only a quarter of the full plate. Because there are two symmetries (x plane and y plane), the geometry can be reduced to 1/4 of the original, simplifying the solution. The domain is then separated into several subdivisions, called "elements". For each element, ANSYS approximates how each element responds to the forces and constraints acting on the domain. For areas where a concentration is likely (i.e. the hole in this situation), the mesh is refined for more accurate results.

Displacement

Okay! Now we can check our solution. Let's start by examining how the plate deformed under the load. Before you start, make sure the software is working in the same units you are by looking to the menu bar and selecting Units > US Customary (in, lbm, lbf, F, s, V, A). Now, look at the Outline window, and select "Total Deformation" under "Solution"

The colored section refers to the magnitude of the deformation (in inches) while the black outline is the undeformed geometry superimposed over the deformed model. The more red a section is, the more it has deformed while the more blue a section is, the less it has deformed. Notice that the deformation is at its highest where the load is applied, and there is no a lot of variation in the y-direction, as one intuitively expect.

Sigma_x

Now lets examine the stress in the x-direction. Look to the Outline window, then click Solution > Sigma-X

From this, you can see that most of the plate is in constant stress, and there is a stress concentration around the hole. The more red areas correspond to a high (positive) stress and the bluer areas correspond to areas of lower (negative) stress. Let's use the probe tool to compare the ANSYS simulation to what we expected from calculation. In the menu bar, click probe; this will allow you to hover over the model and it will display the stress at each point.

Start by hovering over the area far from the hole. The stress is about 200,000 psi, which is the value we would expect for a plate in tension from F/A. If you click the max tag (located next to the probe tool in the menu bar), it will locate and display the maximum stress, which is shown as 6.067E5 psi. This is about a 2.5% difference from the calculation we did in the Pre-Analysis, which is pretty good!

Sigma_r

Now let's look at the radial stresses in the plate. Look to the outline window and click Solution > Sigma-R. This will display the radial stresses.

Does this match what we expect? Let's first look at the case when

. As we found in the pre-calculations,

. This matches the behavior seen in the simulation. From our Pre-Calculations, we also found that

. Using the probe tool, we find that indeed at

the stress is equal to 200,000 psi, which is the value

. From our pre-calculations, we also found that

. Checking the simulation with our trusty probe tool, we find that the ANSYS simulation matches up quite nicely with our calculation.

Sigma_Theta