Legacy elements, such as SOLID45, have a unique output option specified via KEYOPT(6) where surface stress printout is available. The drawback to this output is that it is text only (in the .out file, not the binary .rst file) and only available for legacy elements.

In ANSYS 11.0, a useful feature to evaluate stresses and strains on surfaces of solid elements was added. Instead of associating this output directly with solid elements, one would overlay SHELL181 or SHELL281 on the solid elements’ surfaces of interest (for example, via the ESURF command). If KEYOPT(1)=2 is set for these shell elements, no stiffness or mass matrices will be formed; rather, these shell elements are meant for postprocessing only.

Because surface stresses and strains are output with SHELL181/281 with KEYOPT(1)=2, these shell elements must have the same material properties (constitutive relationships) as the underlying solids (even hyperelasticity is OK!). Also, ensure that a ‘thickness’ is defined (most easily via a real constant definition), which can arbitrarily be set to “1”; otherwise, an error will appear. These elements can be used in nonlinear analyses as well. The element coordinate system (ESYS) specifies the directional output for results in the solution coordinate system (RSYS,SOLU).

Of course, users can postprocess results on the exterior surfaces of solids without these special shell elements; stresses/strains are calculated at the integration points, then copied (or extrapolated) to the nodes. However, use of these special shell elements may provide more accurate stress results since the integration points (1 and 4 for SHELL181 and SHELL281, respectively) lie on the surface. Also, these shell elements can have an element coordinate system oriented independently from the underlying solid elements, allowing for easier output of stresses in a particular direction/orientation (useful if comparing with strain gauge output, for example).