CSTRESS

I/O Options and Subcase Information Entry Used in the I/O Options or Subcase Information sections to request ply stress output for shell elements referencing PCOMP, PCOMPP or PCOMPG properties for all subcases or individual subcases, respectively.

It is also supported for solid elements referencing PCOMPLS or PSOLID with MAT9 for linear static, nonlinear static (both small and large displacement) and nonlinear transient (both small and large displacement) analysis for H3D format.

Format

CSTRESS (format_list,type,random,NDIV,statistics, location) = option

Definitions

Argument Options Description
format <HM, H3D, OPTI, PUNCH, OP2, 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 (.cstr file).
PUNCH
Results are output in Nastran punch results format (.pch file).
OP2
Results are output in Nastran output2 format (.op2 file) 10
HDF5
Results are output in the Hierarchical Data format, Version 5 (.h5 file). 14
blank (Default)
Results are output in all active formats, for which the result is available.
type <ALL, PRINC, TENSOR, DIRECT>

Default = ALL (in DIRECT format)
ALL, blank
All stress results are output.
PRINC
Only principal stress results are output.
TENSOR
All composite stress results are output. Tensor format is used for H3D output.
DIRECT
All composite stress results are output. Direct format is used for H3D output.
random <PSDF, RMS, PSDFC>

No default
PSDF
Requests PSD and RMS 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.
RMS
Requests only the “RMS over Frequencies” result from random response analysis to be output.
Only valid for the 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.
ndiv <INTEGER>

Default = 1

 Number of divisions where composite stresses are calculated. The maximum number of ndiv allowed in the calculation is 5. 9 - 13
statistics <STATIS, OSTATIS, or blank> Composite Stress Statistics over time in a Transient Analysis are controlled by this option. 15
STATIS
Composite Stress Statistics are output in addition to regular composite stress output at each timestep.
OSTATIS
Only the Composite Stress Statistics are output.
blank (Default)
location <CENTER, CORNER, blank>
CENTER (Default)
Results are available at the element center only.
CORNER
Results are available at the element corners and at the element center.
blank
Same as CENTER.

See Comment 16.
option <YES, ALL, blank, NO, NONE, SID, PSID>

Default = YES
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 CSTRESS command is not present, ply stress results are not output.
  2. The STRESS I/O option controls the output of stress results for the homogenized composite material.
  3. 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.
  4. Multiple instances of this card are allowed; if instances are conflicting, the last instance dominates.
  5. The SOUT field on the PCOMP or PCOMPG Bulk Data Entry must be set to YES to activate stress results calculation for the corresponding ply. For PCOMPP, the SOUT field on the corresponding PLY entries should be set to YES.
  6. For plies defined on a PCOMPG Bulk Data Entry, the results are grouped by GPLYID.
  7. For optimization, the frequency of output to a given format is controlled by the I/O option OUTPUT.
  8. format=OUTPUT2 can also be used to request results to be output in the Nastran output2 format (.op2 file).
  9. For shell elements, the following shows the planes where Composite Stresses are calculated for different ndiv values. BOT, MID and TOP represents the bottom, middle and top planes of an individual ply. Division numbers represents the relative distance of a plane/division from the bottom of a ply.
    NDIV
    Planes, where composite strains are calculated
    1
    MID
    2
    BOT, TOP
    3
    BOT, MID, TOP
    4
    BOT, 0.33, 0.67, TOP
    5
    BOT, 0.25, MID, 0.75, TOP


    Figure 1. NDIV Planes of an Individual Ply
  10. If different ndiv values are specified in CSTRESS, CSTRAIN, and CFAILURE, the largest value is used in the composite stress, strain and failure indices calculations.
  11. When CFAILURE is not present, composite strength ratios are not output. CSTRESS and CSTRAIN entries cannot be used to request failure indices.
  12. For shell elements, the NDIV field is supported for linear static, nonlinear static (small and large displacement), normal modes, direct frequency response, modal frequency response, direct transient, modal transient and nonlinear transient (small and large displacement) analysis types only. The NDIV field is supported for first and second order elements.
  13. For solid elements, NDIV is always equal to 3, regardless of the user input.
  14. The HDF5 output is printed to a .h5 binary results file. The current support of HDF5 output format is:
    1. 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.
    2. 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.
    3. In case of Linear Buckling analysis, only DISPLACEMENT result is available in .h5 format.
  15. Composite Stress Statistics are supported for Direct and Modal Linear Transient Analysis types.

    Only H3D output is supported for Composite Stress Statistics.

    The following statistics over time are output for Transient Analysis when STATIS or OSTATIS is specified.
    Statistics
    Supported Composite Stress Result Types
    Minimum and Tme of Minimum
    P1 (Major), P2 (Mid), P3 (Minor), Normal Stresses in Material (Ply) coordinate system
    Maximum and Time of Maximum
    von Mises, P1 (Major), P2 (Mid), P3 (Minor), Normal Stresses in Material (Ply) coordinate system
    Absolute Maximum and Time of Absolute Maximum
    P1 (Major), P2 (Mid), P3 (Minor), Normal Stresses in Material (Ply) coordinate system
    Arithmetic Mean
    Normal Stresses in Material (Ply) coordinate system
    Root Mean Square (RMS)
    Normal Stresses in Material (Ply) coordinate system
    Variance
    Normal Stresses in Material (Ply) coordinate system
    Standard Deviation
    Normal Stresses in Material (Ply) coordinate system

    The Composite Stress Statistics in HyperView can be viewed, after loading the H3D file.

  16. Corner results are available for linear static and nonlinear static (small and large displacement) analysis types only. Currently, only H3D output is supported.