Verification & Validation
It is imperative to do some checks to make sure that the numerical results are accurate. Numerical results can either be compared directly to empirical data or they may be compared to theory.
It should be expected that the structure will experience most of its deformation in the horizontal direction. Additionally, there should be little deformation in the y direction. The results from ANSYS agree with our intuition here.
Another, way to verify the solution of a numerical method is to examine the convergence of the solution as the mesh is refined. Generally, the numerical solution should converge to the exact solution as the mesh is refined. In order to refine the mesh, first expand the mesh tab, , in the tree outline. Next, click on "Edge Sizing", , such that it highlights blue. Now, change the number of divisions in the "Details of "Edge Sizing"" table. Remember, that each line segment of the plane frame structure will be divided in to the number of divisions that you specify. After you have changed the "Number of Divisions" to your preference, click on the solve button, , to recalculate the solution with the new mesh.
The table below displays the outputs of the ANSYS simulation for different meshes.
Number of Elements Per Line Segment
Total Deformation (m)
Force Reactions Verification
From our statics knowledge, we know that the sum of all of the forces needs to be maintained at zero total net force on the structure, or there would be rigid body motion. We can thus add another check that the solution is reasonable by probing the force reactions and checking that in all directions the total forces add to zero:
Probing both of the reactions, we see
From our loading, we have two separate point loads of 4kN each. Then our X-axis balance yields, as we expect
-3988.8N - 4011.2N + 4kN + 4kN = 0
We also have two line pressures of -2kN/m, and with a length of 4m on the two horizontal beams we'd find a total of -16kN of force applied. Our Y-axis balance shows
-16kN + 13218N + 2781.6N = 15999.6N