Coordinate system for stress

Shell stresses are reported at through-thickness integration points. Location of those integration points depend on the number of integration points and the type of integration rule used, e. g., Gaussian, Lobatto, trapezoidal, user-defined rule (see NIP and QR/IRID in *SECTION_SHELL). Fully-integrated shell formulations have 4 in-plane integration points at each through-thickness location. For these formulations, the 4 values of each stress component are averaged before being written.

Shell stresses can be shown in the global, element, or material coordinate systems. By default, shell stresses/strains written to D3PLOT are global; shell stresses/strains written to ELOUT are in the element local coordinate system (except for the case of linear analysis with shell formulations 18,20,21, in which case stresses are in the global system OR when NSOLVR=1 in *CONTROL_IMPLICIT_SOLUTION). Shell stresses/strains from D3PLOT are converted by LS-Prepost to the shell element coordinate system, if you select Toggle > Local axes on from the top menu bar or, alternately, choose E-axes > Local when plotting element time histories or, in the case of fringe plots, switch to Local by clicking on the Glob button at the bottom of the FCOMP menu. The element local coordinate system of a shell is defined as local-x = node 1 to node 2. Local z is normal to the shell.

By default, stresses/strains for solids and thick shells are written to D3PLOT and ELOUT in the global coordinate system. Stresses and resultants for beams are written to D3PLOT and ELOUT in the element coordinate system.

For shells, solids, and thick shells comprised of orthotropic materials, stresses/strains are written to all databases in the material coordinate system if CMPFLG is set to 1 in *DATABASE_EXTENT_BINARY. (Do NOT toggle to local in LS-Prepost if you use this option.) The material coordinate system varies from integration point to integration point within a shell element based on the beta angles given in *SECTION_SHELL.

Summary:

For shells, you can view stresses/strains in the the global coordinate system, in the local element coordinate system (determined solely by element connectivity, i. e., N1-to-N2 is the element x-direction), or (if material is orthotropic and CMPFLG=1 in *DATABASE_EXTENT_BINARY) in the material coordinate system.

For solids or thick shells, you can view stresses/strains in the the global coordinate system or (if material is orthotropic and CMPFLG=1 in *DATABASE_EXTENT_BINARY) in the material coordinate system.