ANSYS 12 - Tensile Bar - Results

Results:

Before we explore the ANSYS results, let's take a peek at the mesh.

Mesh

Click on Mesh (above Solution) in the tree outline.This shows the mesh used to generate the ANSYS solution. The domain is a rectangle. This domain is discretized into a number of small "elements". For each element, ANSYS approximates how the structure responds to the forces acting on the element. A finer mesh is used in areas of greater stress concentration. We have checked that the solution presented  to you is reasonably independent of the mesh.

Displacement:

To view the deformed structure, click on Solution > Displacement in the tree outline. The black rectangle shows the undeformed structure. The deformed structure is colored by the magnitude of the displacement. Red areas have deformed more and blue areas less. You can see that the left end has not moved as specified in the problem statement. This means this boundary condition has been applied correctly. The displacement increases from left to right as we intuitively expect. There is also not much variation in the y-direction. Note the extremely high deformation near the point load. This extremum is unrealistic and should be ignored (there are no point loads in reality).

sigma_x:

Next, let's take a look at the stress components starting with sigma_x. Click on Solution > sigma_x in the tree outline. The stress is uniform away from the ends.

To check what the value is in the uniform region, click on Probe in the toolbar (see snapshot below) at the top and move the cursor on the structure.  Probe values in the middle as well as at the ends. The value of sigma_x away from the ends is nearly 200 MPa (the unit is indicated above the plot). This matches with the P/A value expected from the analytical solution of the equilibrium equations.

In the sigma_x plot, we see that there is deviation from the analytical value in two regions:

•  Around the point load (again the extremely high values very close to the point load are unrealistic).
• At the fixed end.

The analytical solution breaks down in these regions.

sigma_y:

Next, let's take a look at sigma_y. Click on Solution > sigma_y in the tree outline. Again, probe values in the middle as well as at the ends. The value in the middle is close to zero as expected from the analytical solution. There is significant deviation from the analytical solution at both ends.

The analytical method assumed a long bar, therefore by definition, the stresses in the y direction are assumed to be zero. Since this bar does have width, the stresses in the y direction are symmetrical about the middle axis. Note that there are areas where sigma_y is negative. This is a consequence of deformation along the x-axis. Since no extra material is being added, stretching the bar in the x direction would cause a contraction of the bar in the y-direction, and therefore compressive stresses in the y direction.

tau_xy:

 We expect tau_xy to be zero in the middle. Near the ends, since sigma_x and sigma_y are non-zero, we expect

Plot tau_xy, look at the range of values and use Probe to check actual values. Are the above statements valid?

Equivalent Stress (Von Mises):

The Equivalent or Von Mises stress is used to predict yielding of the material. We can consider the maximum and minimum equivalent stresses as the critical design points. We can see that the analytical solution under-predicts the maximum equivalent stress. Thus, one would need to use a large factor of safety if using the analytical result while designing such a structure. One would use a factor of safety with the FEA result also but it does not have to be as large.

[Go To Homework Exercise] 

[See and rate the complete Learning Module]

Go to all ANSYS Learning Modules