CSTRAIN

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

CSTRAIN (format_list,type,random,extras_list,NDIV, location) = option

Definitions

Argument	Options	Description
`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 (.cstr file). PUNCH Results are output in Nastran punch results format (.pch file). OP2 Results are output in Nastran output2 format (.op2 file) 10 PLOT Results are output in Nastran output2 format (.op2 file) when PARAM,`POST` is defined in the Bulk Data section. HDF5 Results are output in the Hierarchical Data format, Version 5 (.h5 file). 15 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 strain results are output. PRINC Only principal strain results are output. TENSOR All composite strain results are output. Tensor format is used for H3D output. DIRECT All composite strain results are output. Direct format is used for H3D output.
`random`	<PSDF, RMS> No default	PSDF Requests PSD and RMS results from Random Response Analysis to be output to the H3D file only. RMS Requests only the “RMS over Frequencies” result from Random Response Analysis to be output.
`extras`	<MECH, THER> 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.
`ndiv`	<INTEGER> Default = 1	Number of divisions where composite strains are calculated. The maximum number of `ndiv` allowed in the calculation is 5. 10 - 14
`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, ALL, blank	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

When the CSTRAIN command is not present, ply strain results are not output.
The STRAIN I/O option controls the output of strain results for the homogenized composite material.
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.
The SOUT field on the PCOMP or PCOMPG Bulk Data Entry must be set to YES to activate strain results calculation for the corresponding ply. For PCOMPP entries, the SOUT field on the corresponding PLY entries should be set to YES.
For plies defined on a PCOMPG Bulk Data Entry, the results are grouped by GPLYID.
For optimization, the frequency of output to a given format is controlled by the I/O option OUTPUT.
The mechanical and thermal contributions to strain may be requested in addition to the total strain.
format=OUTPUT2 can also be used to request results to be output in the Nastran output2 format (.op2 file).
For shell elements, the following shows the planes where Composite Strains 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. For solid elements, ndiv is always 3.

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
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.
When CFAILURE is not present, composite strength ratios are not output. CSTRESS and CSTRAIN entries cannot be used to request failure indices.
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.
For solid elements, NDIV is always equal to 3, regardless of the user input.

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.

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