Command reference help topics

Laminate Random Output Requests dialog box

Note: The laminate dynamic solver writes the number of positive zero crossings and peak results to binary files. To instruct the solver to also write these results to text files, set the Text Output customer default.

Tip:

To find a customer default, choose File tab→Utilities→Customer Defaults, and click Find Default .

Modeling Object
Name	Sets the name for the laminate random output requests modeling object. The name appears in the Output Requests page of the Random Event dialog box.
Properties
The Output Request and Element Selection or Node Selection subgroups appear on all the following pages and the options are almost identical: Accelerations, Displacements, Element Forces, Grid Point Forces, MPC Forces, SPC Forces, Strains, Stresses and Velocities.
Accelerations page
Enable Accelerations Request	Computes acceleration random results if the SOL 103 Real Eigenvalues OP2 file contains displacement results.
Displacements page
Enable Displacements Request	Computes displacement random results if the SOL 103 Real Eigenvalues OP2 file contains displacement results.
Element Forces page
Enable Element Forces Request	Computes element force random results if the SOL 103 Real Eigenvalues OP2 file contains element force results.
Failure Metrics page
Source for Allowables and Failure Theories	Specifies the Nastran OP2 result file for the SOL 103 Real Eigenvalues solution as the source for the material strength and failure theory properties. Note: To use different failure theories or new allowable values, you need to resolve the SOL 103 Real Eigenvalues solution after you modify its settings.
Enable Homogeneous	Computes failure metrics for elements that reference homogeneous materials. The following Homogeneous Output Request options are available.Failure ModeSpecifies the failure mode which can be either Yield or Ultimate. The software uses the value of either yield strength or ultimate strength in the computation of the failure index and the margin of safety.Von Mises StressRequests the output of Von Mises stress results. The software uses the peak Von Mises stress to compute the failure index and the margin of safety.Failure IndexEnables the computation of failure index results for homogenous elements using the following equation:where:F is the failure index.σVM is the peak Von Mises stress.σall is the ultimate or yield strength property of your material. The yield and ultimate strengths are stored in the OP2 file.Margin of SafetyEnables the computation of margin of safety results for homogenous elements using the following equation:where:MS is the margin of safety.FS is the safety factor.Safety FactorSets the safety factor value that is used to compute the margin of safety.Output LocationSpecifies the location at which the software computes stress results. For more information, see the Output Location option in the Output Request group.ElementsSpecifies on which elements the software computes the output results. For more information, see the options in the Element Selection group.		where:F is the failure index.σVM is the peak Von Mises stress.σall is the ultimate or yield strength property of your material. The yield and ultimate strengths are stored in the OP2 file.	where:MS is the margin of safety.FS is the safety factor.
		where:F is the failure index.σVM is the peak Von Mises stress.σall is the ultimate or yield strength property of your material. The yield and ultimate strengths are stored in the OP2 file.
		where:MS is the margin of safety.FS is the safety factor.
Enable Layered	Computes failure metric results for elements that reference a laminate physical property or a solid laminate physical property. The following Layered Output Request options are available.Failure IndexEnables the computation of failure index results for each ply.Strength RatioEnables the computation of strength ratio results for each ply.Margin of SafetyEnables the computation of margin of safety results for each ply.Safety FactorSets the safety factor value that is used to compute the strength ratio and margin of safety.Output LocationSpecifies the location at which the software computes the strain or stress results.See the Output Location option in the Output Request group.ElementsSpecifies the elements on which the software computes the output results. See the options in the Element Selection group.Note: The equations for failure index, strength ratio, and margin of safety depend on the failure theory that you defined in the Laminate Modeler, Layup Modeler, or Solid Laminate Modeler dialog box.
Grid Point Forces page
Enable Grid Point Forces Request	Computes grid point force random results if the SOL 103 Real Eigenvalues OP2 file contains grid point force results. The software can only compute peak results for this quantity.
MPC Forces page
Enable MPC Forces Request	Computes multipoint constraint (MPC) force random results if the SOL 103 Real Eigenvalues OP2 file contains MPC force results.
SPC Forces page
Enable SPC Forces Request	Computes single-point constraint (SPC) force random results if the SOL 103 Real Eigenvalues OP2 file contains SPC force results.
Strains page
Enable Strains Request	Computes strain random results if the SOL 103 Real Eigenvalues OP2 file contains strain results.Note: Laminate Dynamics computes random ply strain results at the same locations that are used for the ply results in the SOL 103 Real Eigenvalues OP2 file. For 3D laminates, before solving your Nastran solution, you define the ply location from the Composite Solid Ply Output list on the Strain page in the Structural Output Requests dialog box.
Stresses page
Enable Stresses Request	Computes stress random results if the SOL 103 Real Eigenvalues OP2 file contains stress results.Note: Laminate Dynamics computes random ply stress results at the same locations that are used for the ply results in the SOL 103 Real Eigenvalues OP2 file. For 3D laminates, before solving your Nastran solution, you set the ply location from the Composite Solid Ply Output list on the Stress page in the Structural Output Requests dialog box.
Velocities page
Enable Velocities Request	Computes velocity random results if the SOL 103 Real Eigenvalues OP2 file contains displacement results.
XY Functions page
The following options specify settings for the abscissa attributes for all XY function requests that you specified on the other pages. Because all requested XY functions are PSD functions, the independent variable is the frequency. These options affect only the format of the output XY plots. They do not have any relation to the frequencies used by the integration algorithms.
Maximum Number of Functions per Request	Sets the maximum number of generated functions for each XY function output request. The functions are stored in the OP2 file of the dynamic simulation. The purpose of this setting is to avoid generating an unmanageable number of XY functions.Example: If you set 5,000 as the maximum number of functions per request, and you request XY functions for displacements and accelerations, the software generates at most 10,000 XY functions in the OP2 file: 5,000 for displacements and 5,000 for accelerations.
Frequency Option	Specifies how the plotting frequencies are generated between the lower and upper bounds. You set the lower and upper bounds in the Random Event dialog box.Linear IncrementsGenerates the plotting frequencies linearly using the number of increments you set in the Number of Increments box.Logarithmic IncrementsGenerates the plotting frequencies logarithmically using the number of increments you set in the Number of Increments box.Between FrequenciesGenerates the plotting frequencies by specifying the number of excitation frequencies between two modal frequencies and the end points (lower and upper frequency bounds). You need to specify the following options to use the Between Frequencies method.Interpolation Between FrequenciesSpecifies linear or logarithmic interpolation between frequencies.Number of Excitation FrequenciesSets the number of excitation frequencies within each subrange including the end points. The first subrange is between the lower bound and the first modal frequency within the bounds. The second subrange is between first and second modal frequencies between the bounds. The last subrange is between the last modal frequency within the bounds and the upper bound.ClusterSets clustering of the excitation frequency near the end points of the range. The cluster value is used to obtain better resolution near the modal frequencies where the response varies the most. A value greater than 1.0 provides closer spacing of excitation frequencies towards both ends of the frequency range, while a value of less than 1.0 provides closer spacing towards the center of the frequency range.
Include Natural Frequencies	Appears when Frequency Option is set to Linear Increments or Logarithmic Increments.Includes the natural frequencies in the plotting frequencies.
Additional Plotting Frequencies	Specifies additional plotting frequencies that will be displayed in the graphs. Typically, add any frequency break points in your input power spectral density function.

Output Request options

Output Request
Peak	Enables the computation of peak values for the requested result set. The peak value is the maximum value that a quantity achieves for the specified confidence level. For a Gaussian distribution: peak value = RMS value x the number of standard deviationsThe following quantities do not follow a Gaussian distribution: Von Mises stresses, some ply failure indices, some ply strength ratios, and some ply margins of safety.Note: Laminate Dynamics computes peak values for all requests, not RMS values even if, in the Post Processing Navigator, some result sets contain the string Root Mean Square in the name, for example, Root Mean Square Acceleration – Nodal.
Positive CrossingsPositive Crossings for Homogeneous Elements	Not available for Grid Point Forces page.Enables the computation of the number of positive zero crossings for the requested result set. The number of positive zero crossings for a response PSD is computed as follows: where:N0 is the number of positive zero crossings.S(f) is the response PSD function.f is the frequency.∫S(f)df is the RMS value for the selected result.The software does not compute the number of positive zero crossings for ply results.		where:N0 is the number of positive zero crossings.S(f) is the response PSD function.f is the frequency.∫S(f)df is the RMS value for the selected result.
		where:N0 is the number of positive zero crossings.S(f) is the response PSD function.f is the frequency.∫S(f)df is the RMS value for the selected result.
XY FunctionsXY Functions for Homogeneous Elements	Not available on the Grid Point Forces page.Enables the generation of the power spectral density functions for the requested result set in the SORT2 format. This allows you to plot the functions from the XY Function Navigator.The software does not compute the XY functions for ply and Von Mises stress results.
Output Location	Available on the Strains, Stresses, and Failure Metrics pages.Specifies the location at which the software computes the requested strain, stress, and failure metric results.CenterComputes the results only at the center of each element.Center and CornerComputes the results at the center and corners of each element. For example, for a hexahedral element, you get results at 9 different locations of each element.

Element or Node Selection options

Element Selection or Node Selection
Elements or Nodes	Specifies the entities on which the software computes the output results. AllComputes requested results on all nodes or elements which have corresponding results in the OP2 file generated by the SOL 103 Real Eigenvalues solution.GroupComputes requested results on nodes or elements that are in the selected group.
Group Reference	Appears when Elements or Nodes is set to Group.Applies the requested output results to the selected group. For more information, see Group Reference options.
Select Object	Appears when Elements or Nodes is set to Group.Lets you select elements or nodes to request the output results on them.Excluded lets you remove individual entities from within your selected object. Note: The Element Selection Filtering options are available when the Type Filter list on the Top Border bar is set to Elements.
Stacked Smart Selector Methods	Opens the Smart Selector Methods dialog box where you can specify a progression of smart selection filters.For more information, see Smart Selector Methods dialog box.

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Laminate Random Output Requests dialog box

Output Request options

Element or Node Selection options

Quick links

Related Topics