I/O Options and Subcase Information Entry The GPSTRESS command can be used in the I/O Options or Subcase Information sections to request grid point stresses output for all subcases or individual subcases, respectively.


GPSTRESS (format_list, averaging, neuber, type, SUBSYS) = option


Argument Options Description
format <HM, H3D, PUNCH, OP2, blank>
Results are output in HyperMesh results format (.res file).
Results are output in Hyper3D format (.h3d file).
Results are output in Nastran punch results format (.pch file).
Results are output in Nastran output2 format (.op2 file). 8
blank (Default)
Results are output in all active formats for which the result is available.
averaging <GLOBAL, BYPROP>

Default = BYPROP

Only the globally averaged GPSTRESS results are output.
BYPROP, blank
Both the globally averaged GPSTRESS results and the GPSTRESS results averaged by property for each property are output.

Default = ALL

Only von Mises stress results are output.
The von Mises and maximum principal stress results are output.
ALL, blank
All stress results are output.
All stress results are output. Tensor format is used for H3D output.
All stress results are output. Direct format is used for H3D output.

No default

ID of the subsystem.

When used along a subsystem definition, this option generates an individual result file for each subsystem with results for that subsystem only.

For more information, refer to the SET Bulk Data Entry.
neuber <NEUBER>

Default = blank

The Grid Point stresses, corrected with Neuber rule are output the H3D file. This is currently only supported for Static analysis. 9
option <YES, ALL, NO, NONE, SID>

Default = ALL

YES, ALL, blank
Grid point stresses output for all elements.
Grid point stresses are not output.
If a set ID is given, grid point stresses are output only for nodes listed in that set.


  1. When a GPSTRESS command is not present, grid point stresses are not output.
  2. Grid point stresses are only available for solid elements.
  3. Grid point stresses are not available for elements which form part of a topology design space. When an analysis only run is performed, grid point stresses are available for all solid elements. When PARAM, REANAL is used, grid point stress contributions are only calculated for fully dense elements.
  4. Multiple formats are allowed on the same entry; these should be comma separated. If a format is not specified, this output control applies to all formats defined by the OUTPUT command, for which the result is available.
  5. Multiple instances of this card are allowed. If instances are conflicting, the last instance dominates.
  6. For optimization, the frequency of output to a given format is controlled by the I/O option OUTPUT.
  7. Grid point stresses are output for the entire model and for each individual PSOLID component. This allows grid point stresses to be accurately obtained at the interface of two components referencing different material definitions.
  8. format=OUTPUT2 can also be used to request results to be output in the Nastran output2 format (.op2 file).
  9. Neuber corrected grid point stresses are calculated based on the Grid point stress from elastic analysis, the Young’s modulus, and the nonlinear material properties defined on the MATS1 Bulk Data Entry. If any grid is located at the junction of two elements of different materials, then the average of the Neuber results of each material is output.