GPFORCE

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

Format

GPFORCE (format_list, elem, form, peakoutput, modal, use) = option

Definitions

Argument Options Description
format <H3D, OPTI, PUNCH, OP2, PLOT, HDF5, blank>

Default = blank
H3D
Results are output in Hyper3D format (.h3d file).
OPTI
Results are output in OptiStruct results format (.gpf file).
PUNCH
Results are output in Nastran punch results format (.pch file).
OP2
Results are output in Nastran output2 format (.op2 file) 9
PLOT
Results are output in Nastran output2 format (.op2 file) when PARAM,POST is defined in the Bulk Data section.
HDF5
Results are output in the Hierarchical Data format, Version 5 (.h5 file). 10
elem (H3D only) <ELEM, NOELEM>
ELEM (Default)
GPFORCE results in the H3D output file includes element contributions.
NOELEM
GPFORCE results in the H3D output file will not include element contributions. However, the TOTAL value for each GRID includes the element contributions.
form <REAL, IMAG, PHASE>

Default = REAL
REAL, IMAG
Provides rectangular format (real and imaginary) of complex output.
PHASE
Provides polar format (phase and magnitude) of complex output.
peakoutput <PEAKOUT>

Default = blank

 If PEAKOUT is present, only the filtered frequencies from the PEAKOUT card will be considered for this output.
modal <MODAL>

Default = blank

 If MODAL is present, grid point forces of the structural modes and residual vectors are output to the PUNCH and OUTPUT2 files for Modal Frequency Response and Transient Analysis.
use <FBD>

Default = blank

 If FBD is present, all the necessary output (SPCFORCE, MPCFORCE, and OLOAD) required for FBD will be triggered automatically.
option <YES, ALL, NO, NONE, SID>

Default = ALL
YES, ALL, blank
Grid point force balance is output for all elements.
NO, NONE
Grid point force balance is not output.
SID
If a set ID is given, grid point force balance is output only for nodes listed in that set.

Comments

  1. When a GPFORCE command is not present, grid point force balance is not output.
  2. GPFORCE output is available for the following solution sequences:
    Solution Sequence
    Output Formats
    Static Analysis
    H3D, OP2, PCH, OPTI
    Normal Modes Analysis
    H3D, OP2, PCH
    Direct Frequency Response Analysis
    H3D, OP2, PCH, OPTI
    Modal Frequency Response Analysis
    H3D, OP2, PCH, OPTI
    Direct Transient Response Analysis
    H3D, OP2, PCH,
    Modal Transient Response Analysis
    H3D, OP2, PCH,
    Nonlinear Transient Response Analysis
    H3D, PCH
  3. The form argument is only applicable for Frequency Response Analysis. It is ignored in other instances.
  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. GPFORCE in .op2 output can only be post-processed with the Free Body Diagram (FBD) tools in HyperMesh/HyperView.
  8. GPFORCE in .h3d output can be used for the Load Transfer Path Analysis with NVH Director. It is only available for Linear Static, Frequency Response, and Acoustic Analyses. An H3D file written with GPFORCE with "use=FBD" (i.e. GPFORCE(FBD)) can be used for FBD in HyperView.
  9. format=OUTPUT2 can also be used to request results to be output in the Nastran output2 format (.op2 file).
  10. The HDF5 output is printed to a .h5 binary results file. The current support of HDF5 output format is:
    1. In case of Linear Static and Normal Modes analysis,
      • The supported element types for element-based results (in .h5 format) are:
        Result Elements Supported
        FORCE/ELFORCE CBAR, CBEAM, CONROD, CTRIA3, CTRIA6, CQUAD4, CQUAD8
        STRESS CROD, CBAR, CBEAM, CONROD, CELAS1, CELAS2, CBUSH, CTRIA3, CTRIA6, CQUAD4, CQUAD8, CTETRA, CHEXA, CPENTA
        STRAIN
      • Corner results are also available for the above results with CQUAD4 and CQUAD8 elements.
    2. In case of Nonlinear Static analysis,
      • The supported element types for STRESS and STRAIN results (in .h5 format) are:
        Result Elements Supported
        STRESS,

        STRAIN

        		 CROD, CELAS1, CBAR, CBEAM, CTRIA3, CTRIA6, CQUAD4, CQUAD8, CHEXA, CPENTA, CTETRA
      • Corner results are also available for CQUAD4 and CQUAD8.
      • DISPLACEMENT, STRESS and STRAIN results are also available on-the-fly during the analysis, if the NLOUT entry is defined in the subcase.
    3. In case of Linear Buckling analysis, only DISPLACEMENT result is available in .h5 format.