STRESS / ELSTRESS
I/O Options and Subcase Information Entry Used to request stress output for all subcases or individual subcases, respectively.
It can also be used to request electric displacement output for Structural Analysis with piezoelectric materials. For more information, refer to Piezoelectric Analysis in the User Guide.
Format
STRESS (sorting,format_list,form,type,location,random,peakoutput,modal, fourier,surf,Neuber, RTHRESH=rthresh, THRESH=thresh, TOP=topn, RTOP=rtop, kpi, psdm,statistics, SUBSYS, NLOUT) = 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.

format  <HM, H3D, OPTI, PUNCH, OP2, PATRAN, APATRAN, PLOT, HDF5, blank> 

form  <COMPLEX, REAL,
IMAG, PHASE,
BOTH> Default (HM only) = COMPLEX Default (all other formats) = REAL 

type  <VON,
PRINC, MAXS,
SHEAR, ALL,
TENSOR, DIRECT> Default = ALL, TENSOR 

location  <CENTER, CUBIC,
SGAGE, CORNER,
BILIN, GAUSS> Refer to Comment 18 and 27 for more information. 

random  <PSDF,
RMS, PSDFC> No default 

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. 
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> 

THRESH  <thresh> Real Default = blank 
Specifies an absolute threshold under which stress results should
not be output. 17 The threshold to exclude elements from stress output is based on von Mises stresses for 2D and 3D elements and on axial stresses for 1D elements. 
RTHRESH  <rthresh> 0.0 < Real < 1.0 Default = blank 
Specifies a relative threshold as a fraction of the maximum von Mises stress under (2D and 3D elements) or maximum axial stress (1D elements) which results should not be output. For example, if VMS is the maximum von Mises stress in the model, the 2D and 3D element 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. The stress values to exclude elements from stress output is based on von Mises stresses for 2D and 3D elements and on axial stresses for 1D elements. 
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. The stress values to exclude elements from stress output is based on von Mises stresses for 2D and 3D elements and on axial stresses for 1D elements. 
kpi  <KPI>
Default = blank 
Key Performance Indicators for stress results are output in the *.kpi ASCII file. 22 
NLOUT  <NLOUT_ID> 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 For more information, refer to Comment 3 in the NLOUT Bulk Data Entry. 
statistics  <STATIS, OSTATIS, or blank>  Stress Statistics over time in Linear Transient Analysis are
controlled by this option. 26

SUBSYS  <SUBSYS_ID> 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. 
option  <YES, ALL, NO,
NONE, SID,
PSID> Default = ALL 

Comments
 When a STRESS command is not present, stress results are output for all elements for all Linear Static Analysis, Nonlinear Quasistatic 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.
However, the SYSSETTING I/O Option Entry (MULTIPLEOUTPUT=YES) can be used in the input file or the Configuration File to request multiple formats of the same output request. For more information, refer to MULTIPLEOUTPUT in the SYSSETTING I/O Option Entry.
 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 fourletter 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, 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 is printed to a .h5 binary results file. For details of the supported analysis types and elements when the .h5 output format is requested, refer to the .h5 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)
 AbsMax
 von Mises, P1 (Major), P2 (Mid), P3 (Minor)
 Time of AbsMax
 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 submenu under Stress Statistics(s).  The default location of stress output can be defined using the OutStress keyword on the OptiStruct configuration file (optistruct.cfg).