ESE

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

Attention: Valid for Implicit and Explicit Analysis

Format

ESE (format_list, type, dmig, extras, neuber, group, creep, peakoutput,THRESH=thresh,RTHRESH=rthresh,TOP=topn,RTOP=rtop, SUBSYS=SUBSYS_ID) = option

Definitions

Argument Options Description
format <HM, H3D, PUNCH, OP2, PLOT, blank>
HM
Results are output in HyperMesh results format (.res file).
H3D
Results are output in Hyper3D format (.h3d file).
PUNCH
Results are output in Nastran punch results format (.pch file).
OP2
Results are output in Nastran output2 format (.op2 file).
PLOT
Results are output in Nastran output2 format (.op2 file) when PARAM,POST is defined in the Bulk Data section.
blank (Default)
Results are output in all active formats for which the result is available.
type <AVERAGE, AMPLITUDE, PEAK>
AVERAGE (Default) 7
In Frequency Response Analysis average energy is output.
AMPLITUDE
In Frequency Response Analysis the amplitude of energy is output.
PEAK
In Frequency Response Analysis the peak energy is output. This is the sum of AVERAGE and AMPLITUDE.
dmig <DMIG, NODMIG>
DMIG
Results are provided for external superelements in the .out file.
If the punch format is specified, DMIG energy is also output to the .pch file, for Linear Static and Normal Modes Analysis only.
NODMIG (Default)
Results are not provided for external superelements in the .out file.
extras <PLASTIC>

Default = blank

Plastic element strain energy is output in addition to total strain). It is only supported for Neuber method in linear static analysis. This output is only available for H3D format.
neuber <NEUBER>

Default = blank

The element strain energy is calculated based on Neuber strain.
group <PROP, COMP, SET, OPROP, OCOMP, OSET> 11

Default = blank

PROP
Group strain energy based on property ID is output. 9
COMP
Group strain energy based on HyperMesh component is output. 9
SET
Group strain energy based on SET with Boolean operator OR is output. This output is available in addition to the elemental strain energy output. 9
OPROP
Only group strain energy based on property ID is output. Elemental strain energy is not output. 9
OCOMP
Only group strain energy based on HyperMesh component is output. Elemental strain energy is not output. 9
OSET
Only group strain energy based on SET with Boolean operator OR is output. Elemental strain energy is not output. 9
creep <CREEP>

Default = blank

CREEP
Strain energy is output in the H3D file. 12
peakoutput <PEAKOUT>

Default = blank

Only the filtered frequencies from the PEAKOUT card will be considered for this output.
THRESH <thresh>

Real

Default = blank

Specifies an absolute threshold under which strain energy results should not be output. 8
RTHRESH <rthresh>

0.0 < Real < 1.0

Default = blank

Specifies a relative threshold as a fraction of the total strain energy under which results should not be output. For example, if TSE is the total strain energy in the model, then strain energy results below TSE*rthresh are excluded from the output.
TOP <topn>

Integer > 0

Default = blank

Only the top, topn, strain energy values should be output.
RTOP <rtop>

0.0 < Real < 1.0

Default = blank

Only the top fraction, rtop, of the total number of strain energy values should be output. For example, if SETOT is the total number of strain energy values in the model, then only the top SETOT*rtop values are output.
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>

Default = ALL

YES, ALL, blank
Element strain energy and strain energy density are output for all elements.
NO, NONE
Element strain energy and strain energy density are not output.
SID
If a set ID is given, element strain energy and strain energy density are output only for elements listed in that set.

Comments

  1. When an ESE command is not present, element strain energy and strain energy density is not output.
  2. Initial thermal strain is included in the calculation of strain energy and strain energy density.
  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. Refer to Results Output by OptiStruct for information on which results are available, in which formats.
  4. Multiple instances of this card are allowed. If instances are conflicting, the last instance dominates.
  5. For optimization, the frequency of output to a given format is controlled by the I/O option OUTPUT. In prior versions of OptiStruct, a combination of the I/O Options FORMAT and RESULTS were used; this method is still supported, but not recommended as it does not allow different frequencies for different formats.
  6. type only applies to Frequency Response Analysis.
  7. The three ways to calculate the element strain energy in Frequency Response Analysis are:
    Output Type
    Formula
    Average
    E 0 = 1 4 ( u r T K E u r + u i T K E u i )
    Amplitude
    E a = 1 4 ( u r T K E u r u i T K E u i ) 2 + ( 2 u r T K E u i ) 2
    Peak
    E peak = E 0 + E a
    Where,
    E
    Corresponding Element Energy
    u r
    Real Part of Displacement
    u i
    Imaginary Part of Displacement
    K E
    Stiffness Matrix
  8. The threshold options (THRESH, RTHRESH, TOP, and RTOP) are available for Static and Frequency 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.).
  9. The group argument is only supported only for Static, Eigenvalue, Frequency Response, Transient Analysis and Aeroelastic Divergence Analysis with H3D and PUNCH formats. In case of Explicit Dynamic Analysis, only COMP and OCOMP group options are available, in the H3D format.
    • In the H3D file, group strain energy and group strain energy density are available under the Element strain energy results type.
    • In the PUNCH file, the Property/Component ID’s and the corresponding strain energy and strain energy density are available.

    If SET/OSET is requested a SID of Boolean SET with operator OR is expected in the field option. Element SETs referenced when using this option should have the OPERATOR field set to OR. Regular element SETs without Boolean OR are not allowed. SET/OSET is currently only supported for H3D and PUNCH formats.

  10. Rotor energy output for Direct/Modal Complex Eigenvalue Analysis (with ASYNC, SYNC, and multiple rotors) is available in the <filename>.rengy file when ESE or EKE output requests are present in the model. The output printed to the .rengy file is calculated as a percentage of the ratio of rotor energy to the requested energy output of elements. It is recommended that you request energy output for ALL elements, so that the rotor energy percentage printed in the .rengy file is meaningful.
  11. Group strain energy is the total energy of all the elements within the group in either PROP, COMP, or SET and group strain energy density is the ratio between the group strain energy and the group volume.
  12. Creep strain energy is supported for both regular H3D (all increments) and _impl.H3D (last increment only) files. Grouping options such as PROP, COMP, and SET are also supported. For a SET output, the SET and CREEP options should be specified. Only OR Boolean SETs are supported. 9
    The following is an example of a SET-based output where creep strain energy for elements in SETs 10, 11, and 12 are output.
    ESE(CREEP,SET,H3D)=25
    	SET,25,ELEM,OR
    +,10,11,12
    	SET,10,ELEM,LIST,
    +,1,2,3
    	SET,11,ELEM,LIST,
    +,19,20,21
    	SET,12,ELEM,LIST,
    +,25,26,27