# Element Results Representation for Models

Elemental results (namely stresses, strains, element forces, flux and gradients) may be provided with reference to either the material system or the elemental system.

For the HM,
PUNCH, and OPTI
output formats, results are provided with
reference to the material system; for first order
shell element results, PARAM,
`OMID` may be used to output with
either representation. The H3D
and OUTPUT2 output formats, to
which these elemental results are written as
tensors, always contain results with reference to
the elemental systems (unaffected by
PARAM,
`OMID`).

Since OptiStruct 10.0 optimization responses always match with the
results written to the HM,
PUNCH, and OPTI
formats and first order shell responses are
consistent with the PARAM,
`OMID` setting.

PSDF and RMS Random Response Stress, Strain results are output in the Element Coordinate system.

## First Order Shell Elements

- With blank
`MCID`/`THETA`(default behavior), stresses, strains and plate forces are presented in the default element material system, which has x-axis aligned with line`G1`-`G2`, and other axis built accordingly to make an orthonormal triad. - With
`MCID`> 0, results are presented in the material system CID projected onto the element plane (projected material system). - With
`MCID`= 0, results are presented in the basic coordinate system projected onto the element plane (projected basic system). - With
`THETA`specified (including zero), results are presented in a rotated element material system, which is rotated by angle`THETA`from the edge`G1`-`G2`.

`G1`-

`G2`system for CTRIA3 elements.

For the H3D and OUTPUT2 formats this representation allows HyperView to perform coordinate system transformations on stress and strain tensors.

## Second Order Shell Elements

The results for second order shells (CQUAD8 and CTRIA6), including shell strains, stresses and forces, are always presented in the local material coordinate system, as described in the manual for CQUAD8 and CTRIA6 elements.

## Composite Shells

Shell-type strains and stresses for composite shells use the same representation as homogeneous
shells. By shell-type results, strains and
stresses calculated at `Z1` and
`Z2` using homogenized shell
properties. Strains and stresses for individual
plies are always presented in the respective ply
coordinate system.

## Solid Elements

- With blank
`CORDM`on the PSOLID card (default behavior), strains and stresses are presented in the basic coordinate system. - With
`CORDM`> 0, strains and stresses are presented in the material system CID. - With
`CORDM`= -1, stresses are presented in the local element coordinate system (described in detail on respective solid element manual pages).

## Gap Elements

For gap elements, gap forces are represented in the gap coordinate system, as described on respective gap element manual pages (CGAP and CGAPG). Compression is positive.