STRAIN

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

Attention: Valid for Implicit and Explicit Analysis

It can also be used to request electric field output for Structural Analysis with piezoelectric materials. For more information, refer to Piezoelectric Analysis in the User Guide.

Format

STRAIN (sorting,format_list,form,type,location,extras_list,random,peakoutput,modal,Neuber, kpi, creep, rate, statistics, RTHRESH=rthresh, THRESH=thresh, TOP=topn, RTOP=rtop, SUBSYS, TOTAL=total, PLASTIC=plastic, NLOUT, NDIV=nlayer) = option

Definitions

Argument Options Descriptions
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. 11
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).
Refer to Strain Results Written in HyperMesh .res Format.
H3D
Results are output in Hyper3D format (.h3d file)..
Refer to Stress Results Written in HyperMesh .res Format.
OPTI
Results are output in OptiStruct results format (.strn file).
The results can be printed in the old or new OPTI format depending on the analysis type. For more information, refer to PARAM, OPTI.
PUNCH
Results are output in Nastran punch results format (.pch file).
Refer to Strain Results Written in Nastran .op2 and .pch Formats.
OP2
Results are output in Nastran output2 format (.op2 file)
Refer to Strain Results Written in Nastran .op2 and .pch Formats). 14
PLOT
Results are output in Nastran output2 format (.op2 file) when PARAM,POST is defined in the Bulk Data section.
Refer to Strain 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 (.h5 file). 18
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>
VON
Only von Mises strain results are output.
PRINC, MAXS, SHEAR
von Mises and maximum principal strain results are output.
ALL (Default)
All strain results are output.
TENSOR
All strain results are output. Tensor format is used for H3D output.
DIRECT
All strain results are output. Direct format is used for H3D output.
location <CENTER, CUBIC, SGAGE, CORNER, BILIN, GAUSS>
CENTER (Default)
Element strains for shell and solid elements are output at the element center only.
CUBIC
Element strains for shell and solid elements are output at the element center and grid points using the strain gage approach with cubic bending correction.
SGAGE
Element strains for shell and solid elements are output at the element center and grid points using the strain gage approach.
CORNER or BILIN
Element strains for shell and solid elements are output at the element center and at the grid points using bilinear extrapolation. 15
GAUSS
Element (Total) strains and plastic strains for shell and solid elements are output at the Gauss integration points. 15
extras <MECH, THER, PLASTIC>

No default

MECH
Output Mechanical strain (in addition to total strain). This output is only available for H3D format.
THER
Output Thermal strain (in addition to total strain). This output is only available for H3D format. 22
PLASTIC
Output Plastic strain (in addition to total strain). This output is only available for H3D format.
random <PSDF, RMS, PSDFC>

No default

PSDF
Requests PSD and RMS results from random response analysis to be output.
RMS
Requests only the "RMS over Frequencies" result from Random Response Analysis to be output.
PSDFC
Requests PSD, RMS and RMS (cumulative) results from random response analysis to be 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, strain results of the structural modes and residual vectors are output to the PUNCH, OUTPUT2 and H3D files for Modal Frequency Response and Transient Analyses.
Neuber <NEUBER>

Default = blank

If NEUBER is present, the von Mises strain corrected using the Neuber rule are output to the H3D file. 16
kpi <KPI>

Default = blank

Key Performance Indicators for Strain results are output in the *.kpi ASCII file. 20
creep <CREEP>

Default = blank

Creep strains are output to the H3D file. 23
rate <RATE>

Default = blank

Strain rate it output to the H3D file. 24
statistics <STATIS, OSTATIS>

Default = blank

Strain statistics over time in linear transient analysis are controlled by this option. 27
STATIS
Strain statistics are output in addition to regular strain output at each timestep for linear transient analysis.
OSTATIS
Only strain statistics are output for linear transient analysis.
blank (Default)
THRESH <thresh>

Real

Default = blank

Specifies an absolute threshold under which strain results should not be output. 28

The threshold to exclude elements from strain output is based on von Mises strain for 2D and 3D elements and on axial strain for 1D elements.

RTHRESH <rthresh>

0.0 < Real < 1.0

Default = blank

Specifies a relative threshold as a fraction of the maximum von Mises strain under (2D and 3D elements) or maximum axial strain (1D elements) which results should not be output. For example, if VMS is the maximum von Mises strain in the model, the 2D and 3D element strain results below VMS*rthresh are excluded from the output.
TOP <topn>

Integer > 0

Default = blank

Only the top topn strain values should be output.

The strain values to exclude elements from strain output is based on von Mises strains for 2D and 3D elements and on axial strains for 1D elements.

RTOP <rtop>

0.0 < Real < 1.0

Default = blank

Only the top fraction ("rtop") of the total number of strains values should be output. For example, if STOT is the total number of strains values in the model, then only the top STOT*rtop values are output.

The strains values to exclude elements from strains output is based on von Mises strains for 2D and 3D elements and on axial strains for 1D elements.

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. 21

For more information, refer to Comment 3 in the NLOUT Bulk Data Entry.

total <YES, NO>
YES (Default)
The total strain tensor is output. 30
NO
The total strain tensor is not output. 30
plastic <YES, NO, EQPS>
YES
The plastic strain tensor is output along with the equivalent plastic strain. 30
NO
The plastic strain tensor and the equivalent plastic strain are not output. 30
EQPS (Default)
The equivalent plastic strain is output. The plastic strain tensor is not output. 30
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.
NDIV <nlayer>

No default

nlayer is the number of layers for shell element results output. A maximum of 50 layers can be defined. The layers are equally distributed over shell thickness direction from bottom to top. The layer results are available in nonlinear implicit analysis only. 29
option <YES, ALL, NO, NONE, SID, PSID>

Default = ALL

YES, ALL, blank
Results are output for all elements.
NO, NONE
Results are not output.
SID
If a set ID is given, results are output only for elements listed in that set.
PSID
If a property set ID is given, results for the elements referencing properties listed in the property set are output.

Comments

  1. When the STRAIN command is not present, no strain data is output.
  2. HyperView can internally derive strain results from the strain tensor when the options TENSOR or ALL are used. If the option DIRECT is used, it will display the strain results that were directly computed.
  3. The von Mises and Principal stress are not available for Frequency Response Analysis.
  4. For elements that reference PCOMP and PCOMPG properties, the STRAIN I/O Option controls only strain results for the homogenized composite. The CSTRAIN I/O Option must be used to obtain ply strain results.
  5. The form argument is only applicable for Frequency Response Analysis. It is ignored in other instances.
  6. The forms BOTH and COMPLEX do not apply to the .frf output files.
  7. 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.
  8. 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.

  9. For optimization, the frequency of output to a given format is controlled by the I/O option OUTPUT.
  10. The mechanical and thermal contributions to strain may be requested in addition to the total strain.
  11. 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.
  12. PSDF and RMS von Mises strain results based on the Segalman Method are also written to the .h3d file for Random Response Analysis (only available in the H3D format).
  13. The four-letter abbreviation STRA is interchangeable with STRAIN.
  14. format=OUTPUT2 can also be used to request results to be output in the Nastran output2 format (.op2 file).
  15. The GAUSS results are currently only supported for H3D and OP2 files. CORNER results are not supported in OPTI format. To display CORNER/GAUSS strain 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** PCH** H3D, OP2**, PCH** H3D, OP2*, PCH* H3D, OP2, PCH
    Corner Strain H3D, OP2, PCH H3D, OP2, PCH H3D H3D, OP2** PCH** H3D, OP2**, PCH** OP2*
    Gauss Stress H3D, OP2 H3D, OP2** H3D, OP2**
    Gauss Strain H3D, OP2 H3D, OP2** H3D, OP2**

    * Only for shell elements.

    ** OP2 and PCH files for NLSTAT and Nonlinear Transient Analysis analysis only include the results at the final timestep.

  16. Neuber corrected strains are calculated based on the von Mises stresses from elastic analysis, the Young's modulus, and the nonlinear material properties defined on the MATS1 Bulk Data Entry. Neuber Strain results are available as elemental results, grid point strains, Gauss point strains, and Corner Neuber strains. Both plastic strain and total strain output are available. Neuber Stress/Strain is supported for Static, Frequency Response, and Transient Analysis for H3D output.
  17. Equivalent plastic strain takes into account the z-component of strain tensor for shells. On the other hand, strain tensor output (even with plastic strain tensor) does not output z-component of strain tensor, which would cause the difference in equivalent plastic strain and von Mises based on plastic strain tensor.
  18. 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.
  19. PSDF and RMS stress results are output in the element coordinate system in H3D file.
  20. KPI output includes maximum value for Strain 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.
  21. nlout=<nloutid> applies only to implicit nonlinear subcases.
  22. If an initial temperature (predefined outside of the subcases) is different from the temperature at the very beginning of a subcase and the resulting thermal expansion is nonzero, the thermal strain due to this temperature difference is counted.
  23. Element based creep strains are output when STRAIN(CREEP,H3D) is specified. If creep strain energy output is required, then ESE(CREEP,H3D) can be used.
  24. Support for strain rate output:
    Nonlinear Static and Nonlinear Transient Analysis
    Either equivalent total strain rate and equivalent plastic strain rate is output depending on TYPSTRT=0 or 1 in MATS1, respectively.
    Explicit Dynamic Analysis
    Both equivalent total strain rate and equivalent plastic strain rate are output.
  25. Only mechanical strain is available for "CBAR/CBEAM Strains". The MECH/THER options are available for "Element Strains (1D)".
  26. Transverse strain is considered in von Mises strain calculation for beam elements.
  27. Strain Statistics are only supported for Direct and Modal Linear Transient Analysis. Only 2D and 3D elements are currently supported.

    Only H3D output is supported for Strain Statistics.

    The following statistics over time are output for Linear Transient Analysis when STATIS or OSTATIS is specified:
    Statistics
    Supported Strain 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 strain statistics in HyperView can be viewed.

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

    Strain Statistics output is also supported for Neuber Strains. For Neuber Strains, the supported components for statistics output are Maximum, Time of Maximum, Arithmetic Mean, RMS, Variance, and Standard Deviation for both Total and Plastic strains.

  28. 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, and so on). Threshold options are also now supported for Neuber Strain. Threshold on Neuber is currently supported only for H3D for static, frequency response, and transient analysis only.
  29. NDIV can be used to output layer results in shell elements. It can control the output of total strain, plastic strain, thermal strain, mechanical strain and equivalent plastic strain in shell elements. When the nlayer is different from the value defined in STRESS or OLOAD, the maximum value of NDIV across the different output requests is taken for output. NDIV is supported for Small and Large Displacement, Implicit Nonlinear Static, and Implicit Transient Analysis.
  30. The TOTAL and PLASTIC options are supported for Implicit Nonlinear Static and Implicit Nonlinear Transient analysis. They are supported for both on-the-fly and regular H3D output files.