Numerical Solution

At this point the items in which we want ANSYS to solve for will be conveyed to ANSYS.

Deformation

It is of interest to have the total deformation, the deformation in the x direction and the deformation in the y direction. In order to solve for the total deformation: (Right Click) Solution > Insert > Deformation > Total.

Now, the two directional deformations will be specified. (Right Click) Solution > Insert > Deformation > Directional. Repeat the instructions in the previous sentence to create a second directional deformation. Next, rename "Directional Deformation" to "X Deformation" and rename "Directional Deformation 2" to "Y Deformation" as shown in the image below. Then, click on "Y Deformation" and change the "Orientation" to the "Y Axis" as shown below.

Stresses, Reaction Forces and Moment Forces

Now, ANSYS will be told to solve for the reaction forces and the reaction moments at the two fixed supports, the direct stress, the minimum combined stress and the maximum combined stress. First (Right Click Solution) > Insert > Beam Tool > Beam Tool.

The stresses will be specified at this point.

(Right Click) Beam Tool > Insert > Beam Tool > Stress > Minimum Bending Stress

(Right Click) Beam Tool > Insert > Beam Tool > Stress > Maximum Bending Stress

The force reactions will be specified now.
Next, (Right Click) Beam Tool > Insert > Probe > Force Reaction. Repeat the steps in the last sentence, in order to create a second reaction force output. Now, highlight "Force Reaction" in the Tree and set the "Boundary Condition" to "Fixed Support" as shown below.

Repeat, this process for "Force Reaction 2", but now assign "Fixed Support 2" to the "Boundary Condition".

Lastly, the moment reactions will be dealt with. (Right Click) Beam Tool > Insert > Probe > Moment Reaction. Repeat the last step to create a second moment reaction. Highlight Moment Reaction in the tree and then set "Boundary Condition" to "Fixed Support" as shown below.

Repeat this process for Moment Reaction 2 and choose "Fixed Support 2" for the Boundary Condition.

Solve

In order to solve, click on the solve button, , which is located near the top of the Setup window. ANSYS will obtain the numerical solution where the ANSYS solver will form the stiffness matrix for each line element, assemble them into the global stiffness matrix and invert it to get the nodal displacements and slopes. It will then extract the requested results and populate the results objects in the tree.