STRESS / ELSTRESS

I/O Options and Subcase Information Entry Used to request stress output for all subcases or individual subcases, respectively.

Format

STRESS (sorting,format_list,form,type,location,random,peakoutput,modal, fourier,surf,Neuber, RTHRESH=rthresh, THRESH=thresh, TOP=topn, RTOP=rtop, kpi, psdm, nlout=nloutid,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) 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. 12 blank (Default) For Normal Modes Analysis, SORT1 is used; 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, PATRAN, APATRAN, PLOT, HDF5, blank>	HM Results are output in HyperMesh results format (.res file). Refer to Stress Results Written in HyperMesh .res Format. H3D Results are output in Hyper3D format (.h3d file). Refer to Stress Results Written in HyperView .h3d Format. OPTI Results are output in OptiStruct results format (multiple files). PUNCH Results are output in Nastran punch results format (.pch file). Refer to Stress Results Written in Nastran .op2 and .pch Formats. OP2 Results are output in Nastran output2 format (.op2 file). 15 Refer to Stress Results Written in Nastran .op2 and .pch Formats. PATRAN Results are output in Patran format (multiple files). APATRAN Results are output in Patran format (multiple files). PLOT Results are output in Nastran output2 format (.op2 file) when PARAM,`POST` is defined in the Bulk Data section. Refer to Stress Results Written in Nastran .op2 and .pch Formats. 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 (.hdf5 file). 20 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 or 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`	<VON, PRINC, MAXS, SHEAR, ALL, TENSOR, DIRECT> Default = ALL, TENSOR	VON Only von Mises stress results are output (HM, OPTI, and H3D only). PRINC, MAXS, SHEAR von Mises and maximum principal stress results are output (HM and H3D only). ALL All stress results are output. TENSOR All stress results are output. Tensor format is used for H3D output. DIRECT All stress results are output. Direct format is used for H3D output.
`location`	<CENTER, CUBIC, SGAGE, CORNER, BILIN, GAUSS>	CENTER (Default) Element stresses for shell and solid elements are output at the element center only. CUBIC Element stresses for shell elements are output at the element center and grid points using the strain gage approach with cubic bending correction. SGAGE Element stresses for shell elements are output at the element center and grid points using the strain gage approach. CORNER or BILIN Element stresses for shell and solid elements are output at the element center and grid points using bilinear extrapolation. 18 GAUSS Element stresses for shell and solid elements are output at the element center and the Gauss integration points. 18
`random`	<PSDF, RMS, PSDFC> No default	PSDF Requests PSD and RMS results from Random Response Analysis to be output for solid and shell elements only. 13 21 Only valid for OUTPUT2 and H3D formats. The "RMS over Frequencies" output is at the end of the Random results in the .h3d file and labeled "Simulation 1" in the .op2 file. RMS Requests only the "RMS over Frequencies" result from Random Response Analysis to be output for solid and shell elements only. 13 21 Valid only for OUTPUT2 and H3D formats. It is labeled "Simulation 1" in the .op2 file. 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.
`PSDM`	<PSDM> Default = blank	If `PSDM` is present, PSD Moments, Number of Peaks and Irregularity Factors for Segalman von Mises stress will be output. For BAR/BEAM elements, axial stress will be adopted instead. Only punch file is supported. 23
`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, stresses of the structural modes and residual vectors are output to the H3D, PUNCH and OUTPUT2 files for Modal Frequency Response and Transient Analysis.
`fourier`	<FOURIER> Default = blank	Stresses output for Modal/Direct Transient Response Analysis with Fourier Transformation. FREQ Frequency domain 24 TIME Time domain 24
`surf`	<SURF> Default = blank	If SURF is present, OptiStruct automatically creates a 2D skin on the outer surfaces of solid elements in the model. The stresses of the skin elements are output based on the selected option.
`Neuber`	<NEUBER> Default = blank	If NEUBER is present, the von Mises stresses, corrected with Neuber rule are output to the H3D file. 19
`mnf`	<MNF, NOMNF>	MNF (Default) Stresses are output to the .mnf file. NOMNF Stresses are excluded from the .mnf file.
`THRESH`	<thresh> Real Default = blank	Specifies an absolute threshold under which stress results should not be output. 17
`RTHRESH`	<rthresh> 0.0 < Real < 1.0 Default = blank	Specifies a relative threshold as a fraction of the maximum von Mises stress under which results should not be output. For example, if VMS is the maximum von Mises stress in the model, then stress results below VMS*rthresh are excluded from the output.
`TOP`	<topn> Integer > 0 Default = blank	Only the top topn stress values should be output.
`RTOP`	<rtop> 0.0 < Real < 1.0 Default = blank	Only the top fraction ("rtop") of the total number of stress values should be output. For example, if STOT is the total number of stress values in the model, then only the top STOT*rtop values are output.
`kpi`	<KPI> Default = blank	Key Performance Indicators for Strain results are output in the *.kpi ASCII file. 22
`nlout`	<nloutid> No default	ID of an NLOUT Bulk Data Entry. If present, the incremental output control parameters are taken from the referenced NLOUT Bulk Data Entry, instead of the one selected by Subcase Entry NLOUT, when results are written into the *_impl.h3d file. 25
`statistics`	<STATIS, OSTATIS, or blank>	Stress Statistics over time in Linear Transient Analysis are controlled by this option. 26 STATIS Stress statistics are output in addition to regular stress output at each timestep for Linear Transient Analysis. OSTATIS Only stress statistics are output for Linear Transient Analysis. blank (Default)
`option`	<YES, ALL, NO, NONE, SID, PSID> Default = ALL	YES, ALL, blank Stress results are output for all elements. NO, NONE Stress results are not output. SID If a set ID is given, stress results are output only for elements listed in that set. PSID If a property set ID is given, stress results for the elements referencing properties listed in the property set are output.

Comments

When a STRESS command is not present, stress results are output for all elements for all Linear Static Analysis, Nonlinear Quasi-static Gap Analysis, and Inertia Relief Analysis subcases.
HyperView can internally derive STRESS results from the stress tensor when the options TENSOR or ALL are used. If the option DIRECT is used, it will display the stress result that were directly computed.
For elements that reference PCOMP or PCOMPG properties, the STRESS I/O Option controls only stress results for the homogenized composite. The CSTRESS I/O Option must be used to obtain ply stress and failure index results.
Only VON, TENSOR and ALL options are accepted for type in Frequency Response Analysis. HyperView can internally derive other STRESS results from the stress tensor for Frequency Response Analysis.
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.
For Normal Modes Analysis output, if there is USET U6 data, the stresses for each residual displacement vector associated with the USET U6 DOF are also output to the H3D, PUNCH, and OUTPUT2 files.
For Modal Frequency Response and Transient Analysis, the stress vectors associated with the residual vectors are written to the .op2 and .pch files after the modal stress vectors if the keyword MODAL is used.
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.
PSDF and RMS von Mises stress results based on the Segalman Method are also written to the .h3d file for Random Response Analysis (only available in the H3D format).
The four-letter abbreviation STRE is interchangeable with STRESS.
format=OUTPUT2 can also be used to request results to be output in the Nastran output2 format (.op2 file).
STRESS(SURF) is not available for EXPDYN solution sequences. OptiStruct will error out, if EXPDYN is the only subcase in the model, and will display a warning message, if there are other subcases in the model, for which STRESS(SURF) can be output. STRESS(SURF) is not available, if neither MAT nor MAT2 are not assigned to the solid materials in the model. Additionally, STRESS(SURF) output is also not available, if MAT1 (with MATS1) is assigned to the elements in the model. Surface shell is not generated if there are only nonlinear materials in the model.
The threshold options (THRESH, RTHRESH, TOP, and RTOP) are available in H3D, OP2, and PUNCH format for Static, Normal Mode, Frequency Response, Transient, and Random Response Analyses only. For H3D, the filter is applied to each dimension of elements (shells, solids, beams, welds, etc.), while for OP2 and PUNCH, it is applied to each element type (quad4, tria3, quad8, etc.).

The GAUSS results are currently only supported for H3D and OP2 files. CORNER results are not supported in OPTI format. To display CORNER/GAUSS stress results in HyperView, activate the Use Corner Results check box in the Contour panel.

CORNER and GAUSS results (Stress, Total Strain, and Plastic Strain) are supported for both Shell (including composite shells) and Solid elements.

	Static	Eigenvalue	Direct Frequency Response	Modal Transient/ Frequency Response	Direct Transient	Nonlinear Static	Nonlinear Transient	Response Spectrum	Random
Corner Stress	H3D, OP2, PCH	H3D, OP2, PCH	H3D, OP2, PCH	H3D, OP2, PCH	H3D, OP2, PCH	H3D, OP2, ² PCH ²	H3D, OP2, ² PCH ²	H3D, OP2 ¹, PCH ¹	H3D, OP2, PCH
Corner Strain	H3D, OP2, PCH			H3D, OP2, PCH	H3D	H3D, OP2, ² PCH ²	H3D, OP2, ² PCH ²	OP2 ¹
Gauss Stress	H3D, OP2					H3D, OP2 ²	H3D, OP2 ²
Gauss Strain	H3D, OP2					H3D, OP2 ²	H3D, OP2 ²

Neuber corrected stresses are calculated based on the von Mises stresses from elastic analysis, the Young's modulus, and the nonlinear material properties defined on MATS1 Bulk Data Entry. Neuber Stress results are available as elemental results, Gauss point stresses, and Corner Neuber stresses. Neuber Strain results are available as elemental results, Gauss point strains, and Corner Neuber strains. Neuber Stress/Strain is supported for Static, Frequency Response, and Transient Analysis for H3D output.
The HDF5 output format is currently supported for the following elements:
- CBEAM, CBAR, CQUAD4, CQUAD8, CTRIA3, CTRIA6, CHEXA, CPENTA, CTETRA, CPYRA (both first and second order) are supported for the listed solid elements.
- The HDF5 output format is currently supported for the following Analysis types:
  Linear Static, Normal Modes, Linear Buckling (only Displacement results are supported for Linear Buckling).
  
  The HDF5 output is printed to an .hdf5 binary results file.
PSDF and RMS stress results are output in the element coordinate system in H3D and OP2 files.
KPI output includes maximum value for Stress with respect to the corresponding property. It is supported for linear and nonlinear static analysis only. Stresses and Strains are supported only for shells and solids. KPI output can also be output for a particular SET using the SID option.
PSDM results are based on Segalman von Mises stress and are output in the Punch file using the following format:

1D/3D Elements

M0, M1, M2, M4, Number of Peaks, Irregularity Factor

2D Elements

Z1, M0, M1, M2, M4, Number of Peaks, Irregularity Factor, Z2, M0, M1, M2, M4, Number of Peaks, Irregularity Factor

For more information on the PSDM output data, refer to Random Response Fatigue Analysis in the User Guide.
The FREQ and TIME options are only valid for Modal/Direct Transient Analysis with Fourier Transformation. When FREQ is present, the displacements in frequency domain would be output in a dummy frequency subcase, which shares the same ID with the transient subcase.
nlout= <nloutid> applies only to implicit nonlinear subcases.
Stress Statistics are only supported for Direct and Modal Linear Transient Analysis. Only Centroid stress is supported and only 2D and 3D elements are currently supported.
Only H3D output is supported for Stress Statistics.

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

Statistics

Supported Stress Result Types

Minimum

von Mises, P1 (Major), P2 (Mid), P3 (Minor)

Time of Minimum

von Mises, P1 (Major), P2 (Mid), P3 (Minor)

Maximum

von Mises, P1 (Major), P2 (Mid), P3 (Minor)

Time of Maximum

von Mises, P1 (Major), P2 (Mid), P3 (Minor)

Abs-Max

von Mises, P1 (Major), P2 (Mid), P3 (Minor)

Time of Abs-Max

von Mises, P1 (Major), P2 (Mid), P3 (Minor)

Arithmetic Mean

von Mises, P1 (Major), P2 (Mid), P3 (Minor)

Root Mean Square (RMS)

von Mises, P1 (Major), P2 (Mid), P3 (Minor)

Variance

von Mises, P1 (Major), P2 (Mid), P3 (Minor)

Standard Deviation

von Mises, P1 (Major), P2 (Mid), P3 (Minor)

After loading the H3D file, the Stress Statistics in HyperView can be viewed.

Various statistics can be chosen from the sub-menu under Stress Statistics(s).

Figure 1.

¹ Only for shell elements.

² OP2 and PCH files for NLSTAT and NLTRAN analysis only include the results at the final timestep.