.articleEntry { font-size:13px; font-weight:normal; line-height:2; } .contributor {color: #000000; font-size:20px; font-weight:bold; }
Debugging Complex Finite Element Analysis Using a Single Element Model
Staff posted on October 14, 2014 |
Save time and headaches with single element analytical testing and other element analysis tips.

By: Peter R. Barrett, P.E., Vice President of CAE Associates

Figure 1 - One Element Model with Symmetry and Imposed Displacement Loading

Trying to get a highly nonlinear finite element analysis to converge is one of the most difficult and frustrating jobs for a finite element analyst. We tend to assume that we correctly input all of the material data and that the software will robustly apply this data to our complex analysis, but that is often not the case!

When running highly nonlinear finite element analyses, users usually bypass the simplest and – very often – most valuable FEA model. Analysts waste a huge amount of time debugging hyperelastic or creep analyses with material models that a single element analytical testing would show are not valid. Creating a one element model seems like a waste of effort, but analysis experts use these all the time. Applications of the single element model include:

• Testing hyperelastic, creep or plasticity material models
• Testing of macros and user-defined material laws
• Quantifying the impact of badly warped elements, aspect ratios and/or skew angles

A single link, beam, 2-d solid, 3-d brick or tetrahedron element model takes seconds to create. Analyzing the same element type proposed in the full analyses illustrates that the material law and convergence controls are valid for this element formulation and the integration settings.

When creating a single brick element for material validation, I prefer to use symmetry boundary conditions on three orthogonal faces to prevent rigid body motion, and not induce any singular stress state. I then ramp on a non-zero displacement on one of the free faces (see Figure 1). This method creates a constant strain and stress state across the element. The use of a ramped displacement loading approach provides a fast and stable solution. The use of a single coupling equation to tie all the non-zero displacement degree of freedom nodes together allows one to postprocess the time history of the force reaction from the coupling equation master node.

When solving a hyperelastic material law where large strains are active, plotting stress vs. strain stored in the results file illustrates the true stress vs. log strain data that can be compared to tests.