Paul Kurowski
President
Acom Consulting

One of the latest methods of slashing development time is to use the 3D models that CAD users create as a basis for finite-element analysis. In a perfect world, performing finite-element analysis on these models directly, rather than recreating data for this purpose, lets analysts concentrate more on analysis and less on syntax.

Solids appear to be a wise choice as a basis for FEA because FE meshing can sometimes take place directly on CAD geometry without modifications. The literature abounds with examples of engineers doing exactly this.

In real life, however, the interface between 3D CAD and FEA is seldom that simple. Solid CAD geometry almost always requires extensive modifications before it is suitable for meshing with finite elements. There also are occasions when solid CAD geometry is completely inappropriate for finite-element models.

Successful interfacing requires time, care, and an understanding of inherent limitations. A few practical examples demonstrate why using unmodified CAD geometry for FEA can lead to erroneous results.

A cooling fin
Consider the task of examining stresses at the vertical base of a horizontal cooling fin after applying bending loads to its edge. The CAD geometry for the fin and a portion of the base plate are exported to an FEA program as a solid and meshed using default parameters in the automesher. An accompanying illustration shows the meshed model and resulting contour plot. But the mesh is not suitable for analysis and results are erroneous. What went wrong?

Automeshing is a purely geometric function. The mesh generator simply fills up the available space with elements because it knows nothing about the expected stress pattern. As a result, it places one or two elements across the fin thickness, many of them poorly shaped by a lack of depth. Considering the kind of elements used (second-order subparametric h-elements), one or even two elements are insufficient to model stress distribution where the fin meets the base. The mesh is incapable of modeling the stress pattern that will develop in the real structure.

This is not a fault of the automesher. Even the best automatic mesh generators provide no assurance of a good mesh. It’s the analyst’s responsibility to make sure the mesh can model a stress pattern according to the laws of mechanics. Several elements are required across the thickness to accurately model bending. However, meshing with greater density would call for a large number of small elements making a prohibitively large FE model. This means the solid CAD geometry is practically unsuitable for meshing with solid h-elements.

Furthermore, insisting on solid CAD geometry locks analysts into using solid elements. The only choice short of running a huge model is to use p-elements which can model bending even with only one element across the fin thickness.

However, p-elements produce a problem which was masked before by the low density of h-elements. The CAD-produced geometry contains reentrant corners, those with more than 180° internal angles, without fillets. A theoretically infinite stress occurs at the corners. P-elements try to model these stresses by increasing the polynomial order of their shape functions. The results reported by a p-element model with singularity depends on the user-required accuracy. As users request greater solution accuracy, the solver responds by increasing the p-order used by elements around the corner. The model reports higher stresses with each increase in p-order. This continues until the solver assigns the highest p-order allowed. Should the user reduce the element size, the situation still repeats itself. Stress in reentrant corners will never converge to a finite value.

In fact, results reported by the model in the illustration are close to results from a shell model discussed later only by coincidence. Had the user employed smaller p-elements or requested a lower convergence error, or both, the model would have reported much higher stresses.

Users must modify CAD-supplied geometry to deal with the inherent sensitivity of p-elements to singularities. For example, users may decide to add small fillets which would always exist in the real structure. The illustration Fin with fillets shows results from a p-element model with added fillets. Alternatively, when looking only for the highest stress, one might analyze a 2D plane strain slice from the middle of the fin, as it appears in the close-up. Of course, this requires modifying the CAD geometry. Another way around the problem of singularities is to recreate the geometry in the FEA program for use with shell elements as in the illustration Fins from shells. Let the geometry consist of planes located in the mid thickness of the original solids. Planes are easily meshed with shell elements which model bending well.

Other examples
Another illustration of difficulties is where a mesher has filled a thin-walled elbow with solid tetrahedral h-elements. This mesh reveals the same fundamental flaws of previous models: only one element placed across the wall and their lack of depth make them poorly shaped.

As in the first example, the mesh generator simply filled up the available space with elements. The automesher has no information on the expected stress patterns and cannot decide how many layers of elements should be placed across the wall. Users must make sure the finite-element mesh is capable of doing what it is asked. With one element across the wall thickness the meshed elbow cannot possibly model the bending which produces the predominant stress.

As before, there are several solutions. One would be to mesh the model with a few solid p-elements. However, it may be more efficient to model the elbow with shell elements even though it means recreating geometry by hand.

A butterfly valve plate illustrates another difficulty. It’s meshed with h-elements to study the stress distribution around the generous fillets transitioning from the central shaft to side plates. The tetrahedral mesh in the illustration has been produced using unmodified CAD geometry. For the same reasons as before, the model is unusable for analysis. In fact, particulars of the butterfly geometry would require many small h-elements resulting in a large time-consuming model. In this case, the valve plate does not lend itself to modeling with shell elements. The only practical choice is to use p-elements. Results shown are based on automatically generated p-elements.

All three examples demonstrate how unmodified CAD geometry may lead to errors in FEA results. Cases where CAD-produced geometry can be used directly for FEA are relatively rare. CAD geometry represents shapes from real life while FEA often requires abstract geometry geared toward analysis. Structurally insignificant details are deleted, thin walls replaced by infinitely thin shells and, in case of symmetry, whole portions of a structure are removed from the finite-element model geometry. It often turns out that, by the time the model is properly prepared, there is little resemblance between CAD geometry and FEA geometry.

Attempts to use CAD geometry directly for FEA often result in huge and expensive models or, worse, in models violating basic laws of mechanics. Implementation of automeshing with p-elements offers less need for analyst judgment and is more likely to produce an acceptable mesh.