ESE

Format

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

Definitions

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

   $E_0=\frac{1}{4}\left({\mathbf{u}}_r^T{\mathbf{K}}_E{\mathbf{u}}_r+{\mathbf{u}}_i^T{\mathbf{K}}_E{\mathbf{u}}_i\right)$

   Amplitude

   $E_a=\frac{1}{4}\sqrt{{\left({\mathbf{u}}_r^T{\mathbf{K}}_E{\mathbf{u}}_r-{\mathbf{u}}_i^T{\mathbf{K}}_E{\mathbf{u}}_i\right)}^2+{\left(2{\mathbf{u}}_r^T{\mathbf{K}}_E{\mathbf{u}}_i\right)}^2}$

   Peak

   $E_{\mathit{peak}}=E_0+E_a$

   Where,

   $E$

   Corresponding Element Energy

   ${\mathbf{u}}_r$

   Real Part of Displacement

   ${\mathbf{u}}_i$

   Imaginary Part of Displacement

   ${\mathbf{K}}_E$

   Stiffness Matrix

8. format=OUTPUT2 can also be used to request results to be output in the Nastran output2 format (.op2 file).
9. 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.).
10. The group argument is only supported only for Static, Eigenvalue, Frequency response, and Transient analysis in H3D and PCH format. Group Strain Energy and Group Strain Energy Density are available under the Element Strain Energy results type in the H3D file. 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.

11. 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.
12. 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.