Argument

Options

Description

sorting

<SORT1, SORT2>

Default = blank

This argument only applies to the PUNCH format (.pch file) or the OUTPUT2 format (.op2 file) output for normal modes, frequency response, and transient subcases. It will be ignored without warning if used elsewhere.

SORT1:

Results for each frequency/timestep are grouped together.

SORT2:

Results for each grid/element are grouped together (Comment 8).

blank:

For frequency response analysis, if element SET is not specified, SORT1 is used, otherwise, SORT2 is used; for transient analysis, SORT2 is used.

format

<HM, H3D, OPTI, PUNCH, OP2, PLOT, blank>

Default = blank

HM:

Results are output in HyperMesh result format (.res file).

H3D:

Results are output in Hyper3D format (.h3d file).

OPTI:

Results are output in OptiStruct results format (.force file).

PUNCH:

Results are output in Nastran punch results format (.pch file).

OP2:

Results are output in Nastran output2 format (.op2 file) (Comment 11).

PLOT:

Results are output in Nastran output2 format (.op2 file) when PARAM, POST is defined in the bulk data section.

If PARAM, POST is not defined in the bulk data section, this format allows the form for complex results to be defined for XYPUNCH output without having other output.

blank:

Results are output in all active formats for which the result is available.

form

<COMPLEX, REAL,
IMAG, PHASE,
BOTH>

Default (HM only) = COMPLEX

Default (all other formats) = REAL

COMPLEX (HM only), blank:

Provides a combined magnitude/phase form of complex output to the .res file for the HM output format.

REAL, IMAG:

Provides rectangular format (real and imaginary) of complex output.

PHASE:

Provides polar format (phase and magnitude) of complex output.

BOTH (HM only):

Provides both rectangular and polar formats of complex output.

type

<TENSOR, DIRECT>

Default = TENSOR

TENSOR:

Force results are output for all solution sequences in which force results are supported. The Tensor format is used for H3D output (Comment 9).

DIRECT:

Force results are output for all solution sequences in which force results are supported. The Direct format is used for H3D output (Comment 9).

location

<CENTER, CUBIC, SGAGE, CORNER, BILIN>

Default = CENTER

CENTER:

Element forces for shell and solid elements are output at the element center only.

CUBIC:

Element forces for shell elements are output at the element center and grid points using the strain gage approach with cubic bending correction.

SGAGE:

Element forces for shell elements are output at the element center and grid points using the strain gage approach.

CORNER or BILIN:

Element forces for shell elements are output at the element center and at the grid points using bilinear extrapolation.

random

<PSDF, RMS>

No default

PSDF:

Requests PSD and RMS results from random response analysis to be output for CBUSH elements only.

Only valid for H3D format. The "RMS over Frequencies" output is at the end of the Random results in the .h3d file.

RMS:

Requests only the “RMS over Frequencies” result from random response analysis to be output for CBUSH elements only.

Valid only for the H3D format.

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

MODAL:

If MODAL is present, element forces of the structural modes and residual vectors are output to the PUNCH and OUTPUT2 files for modal frequency response and transient analysis.

option

<YES, ALL, NO,
NONE, SID>

Default = ALL

YES, ALL, blank:

Element force is output for all valid elements. If fluid elements are present, then Fluid Particle Velocity is output for all fluid elements in the model.

NO, NONE:

Force or Fluid Particle Velocity is not output.

SID:

If a set ID is given, force is output only for valid elements listed in that set. If the set contains Fluid elements, then Fluid Particle Velocity is output for the corresponding Fluid elements.