In producing a line- or banded-type contour plot of an element-based field output variable, such as stress or strain, Abaqus/Viewer (or any other post-processor) extrapolates the output variable from the integration points of each element to the nodes of each element. A conditional averaging process is used at each node to account for contributions from surrounding elements. The averaged nodal values are used in the contour plot. In general, the accuracy of the averaged nodal values as compared to the integration point values will depend on the severity of gradients in the region and the density of the mesh.
Reduced integrated linear hex elements have 1 integration point per element only and the nodal results are identical to the integration point results. Fully integrated linear and quadratic elements (tet or hex shape) have multiple integration points and extrapolation will take place (see another blog).
The extrapolation of the results becomes harder to interpret, when you have large gradients of the solution over an element. If the model contains a material capable of deforming plastically, the integration point stresses are calculated from the plastic constitutive equation. The satisfaction of the plastic constitutive law is not enforced on the extrapolated stresses. The extrapolation and averaging process may result in Mises stresses that are reported to be higher or lower than the material’s actual ultimate stress.
As an example, imagine that for a specific element the most outside integration point just reaches plasticity (stress is 100 [MPa], plastic strain is 0.01 %), while the integration point further away from the surface remains in the elastic domain (stress is 50 [MPa], plastic strain is 0%). Depending on the element shape, it is possible that due to extrapolation an element node obtains a stress value of 150 [MPa] which may be larger than the specified ultimate stress of the material. At the same time the extrapolation of the plastic strain may lead to a result of 0.02% on the same element node. This value may not correspond to the extrapolated value of the stress based on the material constitutive law.
For reduced integration linear hex elements, stresses and strains may be underestimated due to lack of extrapolation of the integration point results to the nodes. For other elements, stresses and strains may be overestimated due to the extrapolation and one should be extra careful when plasticity occurs. Results from all different element types will converge to the same (and “correct”) result when the mesh is refined, and the gradients become more accurately represented.
‘Skin’ technique of volumetric components
A widely used workaround for the above described extrapolation issue, is the so-called ‘skin’ technique of volumetric components. With this technique very thin membrane elements are added to the outside of the volumetric mesh, sharing the nodes with the underlying brick and/or tet elements. The stress and strain results in the membrane elements represent the actual stress and strain on the outside of the component and are not affected by extrapolation.
Below you can find a video how you can create skins in Abaqus.