FORCE / ELFORCE

I/O Options and Subcase Information Entry Used to request structural element force output and elemental fluid particle velocity output for all subcases or individual subcases, respectively.

Format

FORCE (sorting, format_list, form, type, location, random, peakoutput, modal,statistics) = option

Definitions

Argument	Options	Description
`sorting`	<SORT1, SORT2>	This argument only applies to the PUNCH format (.pch file) or the OUTPUT2 format (.op2 file 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. 8 blank (Default) 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, HDF5, blank>	HM Results are output in HyperMesh results 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). 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. HDF5 Results are output in the Hierarchical Data format, Version 5 (.h5 file). 13 blank (Default) 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>	TENSOR (Default) Force results are output for all solution sequences in which force results are supported. The Tensor format is used for H3D output. 9 DIRECT Force results are output for all solution sequences in which force results are supported. The Direct format is used for H3D output. 9
`location`	<CENTER, CUBIC, SGAGE, CORNER, BILIN>	CENTER (Default) 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, PSDFC> 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. Only valid for H3D format. PSDFC Requests PSD, RMS and RMS (cumulative) results from random response analysis to be output. Only valid for the H3D format. The "RMS over Frequencies" output is at the end of the random results.
`peakout`	<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.
`statistics`	<STATIS, OSTATIS, or blank>	Element force statistics over time in a Transient Analysis are controlled by this option. 14 STATIS Element force statistics are output in addition to regular element force output at each timestep. OSTATIS Only the Element force statistics are output. blank (Default)
`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.

Comments

If neither FORCE nor ELFORCE commands are present, then Force results or Fluid Particle Velocity results are not output. Fluid Particle Velocity results are currently only supported for H3D, OP2, and PUNCH formats.
FORCE results are available for ELAS (CELAS1, CELAS2, CELAS3, CELAS4), ROD (CROD), BAR (CBAR, CBEAM), BUSH (CBUSH), PLATE (CQUAD, CTRIA), GAP (CGAP), FASTENER (CFAST)*, VISCOUS DAMPER (CVISC), SCALAR DAMPER (CDAMP1, CDAMP2, CDAMP3, CDAMP4) and WELD (CWELD) elements.
*CFAST elements or their corresponding force results are available for post-processing in HyperView only if the .fem file is loaded as a model. 9
The form argument is only applicable for Frequency Response Analysis. It is ignored in other instances.
The forms BOTH and COMPLEX do not apply to the .frf output files.
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.
Multiple instances of this card are allowed; if instances are conflicting, the last instance dominates.
For optimization, the frequency of output to a given format is controlled by the I/O option OUTPUT.
In general, HyperView does not recognize the SORT2 format for results from the .op2 file. When results are output only in SORT2 format (<Result Keyword> (SORT2, OUTPUT2, ...)), the results are written by OptiStruct into the .op2 file in SORT2 format, but when the .op2 file is imported into HyperView, the results in SORT2 format are not recognized. Therefore, the SORT1 option is recommended for results output in OUTPUT2 format and SORT2 option is recommended for results output in PUNCH format.
Vector and Tensor plots of some element force results (weld, beam/bar and gap elements) are available for post-processing in HyperView only if the .fem file is loaded in the Load model field and the results file is loaded in the Load results field (Figure 1 is an example illustration of the HyperView Load model and results panel).
Make sure that the Advanced option is selected from the Result Math template: menu.

Figure 1.
For shell elements force results are given as force/unit length.
format=OUTPUT2 can also be used to request results to be output in the Nastran output2 format (.op2 file).
For Fluid velocity output, the Real and Imaginary parts are calculated as:
(1)
$v_{x}^{R} = - \frac{1}{ρ ω} \frac{\partial p^{I}}{\partial x}$
(2)
$v_{x}^{I} = \frac{1}{ρ ω} \frac{\partial p^{R}}{\partial x}$

Where,

$ρ$

Fluid density

$p$

Acoustic pressure

$ω$

Frequency

$v_{x}^{R}$

The Real part of the Fluid Velocity along the X-axis

$v_{x}^{I}$

The Imaginary part of the Fluid Velocity along the X-axis

The Fluid Velocities in other directions (Y and Z) can be calculated similarly. Fluid velocity output in Coupled Frequency Response Analysis (Acoustic Analysis) refers to an elemental quantity and not a nodal/grid-based value.

The HDF5 output is printed to a .h5 binary results file. The current support of HDF5 output format is:

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.

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.

In case of Linear Buckling analysis, only DISPLACEMENT result is available in .h5 format.

Element force statistics are supported for Direct and Modal Linear Transient Analysis.
Only H3D output is supported for element force statistics and the output is available only for the following elements - CBAR, CBEAM, CELAS1, CELAS2, CONROD, CROD, CBUSH, CVISC, CDAMP1, CDAMP2, CGAP, CWELD, CGAPG and CSEAM.

The following statistics over time are output for Transient Analysis when STATIS or OSTATIS is specified.

Statistics

Supported Element Force Result Types

Minimum and Time of Minimum

X-component, Y-component, Z-component

Maximum and Time of Maximum

Magnitude, X-component, Y-component, Z-component

Absolute Maximum and Time of Absolute Maximum

Magnitude, X-component, Y-component, Z-component

Arithmetic Mean, Root Mean Square (RMS), Variance, and Standard Deviation

Magnitude, X-component, Y-component, Z-component

The Element Force statistics can be viewed in HyperView after loading the H3D file, under Statistics over time option at the end of the timestep list in the Results Browser. Then, various statistics can be chosen from the sub-menu under Element Forces (1D) (Statistics) (s).

Figure 2.