If one model has been subject to a convergence study, as described in the first article, then it would be logical to argue that the corresponding region in a model of a ‘similar’ structure, with the same level of mesh refinement, would have the same level of accuracy. This is true, providing the ‘similarity’ of models includes similarity in stress gradients.
Often, strengthening a region of a structure can attract more load and produce higher stresses in fillets or other features, requiring careful detail design and analysis. The strengthened structure in this case is not ‘similar’ to the previous design in that it will have higher stress gradients, requiring an increase in mesh density in this region, to give comparable accuracy with analysis of the previous design. This is especially important as the stresses tend towards the limiting strength of the material, and become critical to the acceptance of the new design.
Even without design changes to the structure, a simple increase in load magnitude means that stress gradients will be increased in certain regions. Although the accuracy as a percentage of peak stress will not change, the accuracy relative to the yield stress of the material will be reduced, unless the mesh is refined.
Using Element Size as a Measure of Convergence
In light of the previous discussion, it will be obvious that assuming a mesh is convergent for stress just because it has the same element size as a converged mesh in a non-similar model, or in a different location in a similar model, is not valid.
Stress accuracy will depend on element size to some extent, but the element’s proximity to a stress concentration or the variation of the load in the structure in the region of interest is more important.
The figure opposite shows a 2D or 3D mesh region, representing an internal corner. No radius is modelled. An internal corner with zero radius like this could have an infinite theoretical stress, if made from a perfectly elastic material. This is not to do with any numerical effects of FEA but because the stress concentration in most situations is infinite for this geometry.
As the mesh is refined, the stress will increase without limit. Thus, the stresses predicted by an FE analysis of a fillet modelled in this way is only dependant on the size of the elements and has nothing to do with any real values that might occur there.
Quite often, sensible stresses can be predicted from representing an internal fillet in this way but that doesn’t mean they are valid; the actual radius specified in the drawing must be represented with a suitable number of elements spaced around the fillet, to achieve a predictable elastic stress. (There could be serious implications if the drawing specifying this feature does not include a minimum radius.)