Sign-up for free online course on ANSYS simulations!Unable to render {include} The included page could not be found.
Step 7: Verification & Validation
Importance of Verification
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.
Verification of Maximum Bending Stress and Maximum Total Deformation
The ANSYS results will be verified by comparing them to the results obtained using Euler-Bernoulli beam theory in the pre-analysis. The ANSYS simulation outputted 4.6352MPa for the maximum bending stress and the calculation in the pre-analysis yielded 4.635 MPa. The ANSYS simulation outputted 0.0051352m for the total deformation of the beam at x=4 while the calculation from the pre-analysis yielded 0.005103m. The ANSYS results very closely match the calculations from the pre-analysis, thus the simulation has been verified.
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. The table below displays the outputs of the ANSYS simulation for a mesh of 2 elements and a mesh of 10 elements.
|
Total Deformation (m) |
Maximum Bending Stress Pa |
|---|---|---|
Theory Values |
0.005103 |
4.635x10^6 |
2 Element FEA |
0.0051352 |
4.6352x10^6 |
10 Element FEA |
0.0051352 |
4.6352x10^6 |
As one can see from the table above the results do not change as the mesh is refined. The reason that the results do not change is that they have already converged to the answer. The exact solution for the deformation is cubic and for this setup ANSYS uses element BEAM 188 which in turn uses cubic interpolation. Thus, for the simple cantilever beam setup the numerical method converges very quickly.
Go To Exercises