Even before you mesh a part, you may have introduced the potential for erroneous stresses and deflections.

**Paul Kurowski**President

Design Generator Inc.

London, Ontario, Canada

Edited by Paul Dvorak

Every day brings news of powerful analysis software for shortening development cycles. Trying to keep pace with such progress makes it easy to forget that all those great programs provide accurate results only when properly used.

One of the stumbling blocks on the road to quick and correct FEA results includes idealization errors, those that come from simplifying the real world. They are common yet often unrecognized and dangerous. In this discussion of them, lets use the term finite-element method (FEM), the foundation of FEA, because it emphasizes the underlying numerical method.

It's also useful to briefly review the four steps present in any FEM project. Step one transforms boundary conditions, material properties, and geometry into terms acceptable for analysis. Simplifications are almost always necessary, but they introduce idealization errors. Some are benign but others are hazardous. And don't be too smug if you're using "advanced" software because idealization errors have nothing to do with mesh, elements, or the type of solver used.

Mathematical models formed by simplifications and containing idealization errors then take the form of differential equations. These are usually too difficult to solve analytically, so solvers use an approximate numerical method. Most often we choose the FEM, which has dominated engineering analysis because of its adaptability and numerical efficiency. FEM requires splitting the continuous model into discrete regions or elements. Call this step two, another operation with opportunity for errors.

Step three, the solution, leaves little opportunity for user intervention. The software can introduce numerical round-off errors, but recent programming minimizes their impact.

And in step four, after solving a model, you apply results to the design. At that time, it's important to recall the assumptions made during the simplifications and meshing because they have influenced the results.

The boxes that follow show several particular idealization errors that are introduced in step one. And the article avoids referencing FEM-specific issues, such as elements and meshing, as much as possible. However we must touch on the convergence process and the idea of degrees-of-freedom in FEM models because we'll use those as tools to expose the problems of idealizations. To illustrate the convergence process, the examples that follow are meshed and solved with a program that uses p-elements, but the problems they illustrate apply to all FEM-based analysis or any other kind of numerical analysis for that matter.

A classic problem involves finding the maximum principal stress in a plate with a center hole. Two-dimensional plane stress is assumed. Results show the highest stress equal to 377 MPa, quite close to 370 MPa predicted by the analytical solution. But 377 MPa is Large elements, such as those in
So you might ask: Which model is correct, We should emphasize that our plate with the center hole illustrates benign idealization errors introduced in by a rigid support. We had to hunt for singularities and use the trick of very small elements and nonadaptive convergence to reveal them. Benign singularities are common and practically unavoidable. Even the following test bracket is not free from them. In practice, we either don't notice pesky stress concentrations or learn to ignore them, but it is still worthwhile to remember about occasional troubles caused by Mr. Poisson and his ratio. |

A curved I-beam it is easy, yet deadly, to forget that buckling, not the stress, will define the structure's safety. With a little work, we could fill this entire issue with examples of modeling errors introduced during the idealization process. Indeed, reducing 3D models to 2D representations, beam and shell modeling, defeaturing and geometry clean up, all that is done to simplify models and allow meshing. Each process abounds in traps awaiting an unsuspecting user. Modeling errors originate from incorrect mathematical models. Some modeling errors, such as singularities, can be revealed (but not cured) using the FEM-based convergence process. Most remain hidden. The only defense is full understanding of the analyzed problem. |

The next objective is to analyze a deflection in the model in Small-displacement theory assumes membranes don't change stiffness as they deform and so it accounts only for the initial bending stiffness. However, the material under deformation acquires "membrane stiffness", which adds to the original value for bending stiffness. As a result, the overall stiffness increases as the membrane deforms. A nonlinear-geometry analysis, also called large-deformations analysis, is required even though the displacement magnitude seems small. The difference between results returned by linear and nonlinear models appears in the red and blue graph. |

Idealization errors are not always mild. They often lead to hazardous situations. For example, find the maximum principal stress in a simple 2D plane-stress model for an L-shaped bracket. The As revealed by the convergence process, reducing element size and upgrading element order lets us chase infinity — 415 MPa is just as far away from infinity as 79 MPa. This time we can't ignore the singularity and still produce meaningful results because we are interested in stress in the location where it's singular. The remedy is to change the model. One way is to add a fillet, which is always present in real parts anyway. You can also avoid stress singularities by using a different material model, for example the elasticplastic model instead of a linear-elastic material. The elastic-plastic material model would put an upper bound on stress, and instead of producing meaningless high stress, a plasticity zone would be formed. Geometric details, such as a fillet, are frequently difficult to mesh. A technique called defeaturing removes such offending geometry to simplify meshing. Defeaturing, however, can be dangerous. Take the Convergence should determine whether or not the results are significantly discretization dependent. Only when results converge can we use them with confidence to make design decisions. The L-shape bracket demonstrates the opposite: results are entirely discretization dependent and completely meaningless. |

Singularities can also affect displacements. Imagine a beam in bending supported at one end by two welds, as in A stress convergence curve (not shown) reveals a problem: The curve is not converging. Clearly, this model is not useful for stress analysis because stresses are discretization dependent, that is, they are singular. Notice again that the error in definition of the math model is revealed by the convergence curve. Looking at results of just one single run would have been misleading. So a useful stress analysis is out of the question. But can we use the model for deflection analysis? Instead, it's slowly but surely increasing. How is that possible? Point supports at the corner show stress that tends to infinity. In fact, the strain also tends to infinity. After all, it is proportional to stress. (The linear relation between stress and strain is expressed by Hooke's law, or = The model in One can conclude that both types of modeling errors (sharp re-entrant corners and point supports) originate from an improper definition of the mathematical model upon which the FEM model is constructed. But the errors have nothing to do with FEM. We committed them in step one |

**A FINAL WORD ON CONVERGENCE**

The convergence process adds degrees of freedom to the FEM model to see how results change. Degrees of freedom are added either by using more elements (mesh refinement, called h convergence), or by using higher-element orders (p-convergence).

Convergence should demonstrate that results converge to a finite value and, therefore, are not significantly dependent on the choice of discretization. If the process shows that results are significantly discretization dependent, then the results are unreliable.

**STEPS IN FEM PROJECT**Step 1 Simplifications of reality lead to a mathematical model and introduce idealization errors.

Step 2 Replacing a continuum with a set of discrete regions (meshing) introduces discretization errors.

Step 3 The solution of a discrete system introduces numerical errors.

Step 4 Analysis of results introduces interpretation errors.