Structural, FRF, and Thermal Output Requests dialog boxes (Nastran)

Common options

Modeling Object
Name	Sets the name of the modeling object.
Label	Sets a unique numerical identifier for the modeling object.
Properties
Description	Enter a brief description or click to open a text editor where you can enter a longer description.
Preview	Opens an information window where you can examine all current output requests and their options.
Enable All	Selects all output requests.
Disable All	Clears all output requests.
Output request options
Sorting	Specifies the case control command option that requests the format of printed output.SORT1Requests the output of results as a tabular listing of the selected output for each node in each individual subcase.SORT2Requests the output of results as a tabular listing of the subcases for each selected output option.DefaultChooses the default option for your analysis type. For example, SORT1 is the default in static analysis, while SORT2 is the default in transient response analysis.
Output Medium	Specifies the case control command option that requests the output destination for the results.PRINTRequests the output of results to the printer.PUNCHRequests the output of results to the .pch (ASCII format) file.PRINT,PUNCHRequests the output of results to the printer and the .pch (ASCII format) file.PLOTReports the output of results to the .op2 file.See Simcenter Nastran Output Files in the Simcenter Nastran User's Guide for more information.
Data Format	Specifies the case control command option that requests the format of complex output.REALRequests the real and imaginary output in rectangular format.IMAGFor most solutions, IMAG = REAL.PHASERequests the magnitude and phase output in polar format.Note: See case control command remarks in the Simcenter Nastran Quick Reference Guide to check if your solution supports IMAG and PHASE.
Entity Selection	Depending on the individual case control command, specifies options to control the location where the software outputs results.ALLSelects all entities.GroupIf you choose Group, select the appropriate node or element set.NONELets you turn this output request off; useful for controlling output requests across subcases.Note: For Grid, Modal, and Panel Contribution case control commands in the Output Requests dialog box, you can select the following options for a response contribution set. The response contribution set produces output that relates the response at specified locations at each excitation frequency to nodes (grids) in structural panels, structural or fluid modes, or structural panels:SpecifyLets you create or select a response contribution set.NONELets you turn this output request off; useful for controlling output requests across subcases.
Node Selection	Group ReferenceApplies the requested output results to the selected group. For more information, see Group Reference options.Select Object Lets you select the geometry or FE entities to request the output results on them.Note: The Node Selection Filtering options are available when the Type Filter list on the Top Border bar is set to Nodes.

Structural Output Requests options

Properties
Solution Applicability View	Filters the dialog box to display only solution-specific case control commands. When you select a filter, the dialog box displays all case control commands for the selected solution type.This list supports the most common solution types.
Output request options
Enforced Motion Output	Specifies the case control command option that requests the format of velocity results.ABSRequests absolute velocity output.RELRequests output relative to the enforced motion output.DefaultChooses the default format option for velocity results.Note: See case control command description in the Simcenter Nastran Quick Reference Guide to determine the default value.
Random Output Medium	Specifies the case control command option that sets the output destination for random results.RPRINT (Default)Outputs the results to the printer.RPRINT,RPUNCHOutputs the results to the printer and the .pch (ASCII format) file.NORPRINT,RPUNCHDoes not output results to the printer, but reports the results in the .pch (ASCII format) file.NORPRINTDoes not output results to the printer.See Simcenter Nastran Output Files in the Simcenter Nastran User's Guide for more information.
Random Functions	Specifies the case control command options that request the calculation of specific random functions.SpecifyLets you select:PSDFRequests the calculation of the power spectral density function.ATOCRequests the calculation of the autocorrelation function.CRMSRequests the calculation of the cumulative root mean square function.RMSRequests the calculation of the root mean square and zero crossing functions.Note: See case control command remarks in the Simcenter Nastran Quick Reference Guide to check if your solution supports all the above options.RALLRequests the calculation of PSDF, ATOC, CRMS, and RMS.DefaultChooses the default random function option.Note: See case control command description in the Simcenter Nastran Quick Reference Guide to determine the default value.Note: For Cross-Power Spectral Density/Cross-Correlation Function case control command in the Output Requests dialog box, you select the options:PSDFRequests the calculation of the cross-power spectral density function.CORFRequests the calculation of the cross-correlation function.RALLRequests PSDF and CORF.
Acceleration
Enable ACCELERATION Request	Enables the ACCELERATION case control command to request acceleration vector output.
Applied Load
Enable OLOAD Request	Enables the OLOAD case control command to request applied load vector output.
Contact Result
Enable BCRESULTS Request	Enables the BCRESULTS case control command to request contact results output.
Pressure	Specifies the TRACTION option on the BCRESULTS case control command.
Force	Specifies the FORCE option on the BCRESULTS case control command.
Displacement
Enable DISPLACEMENT Request	Enables the DISPLACEMENT case control command to request displacement output.
Elastic Strain
Enable ELSTRN Request	Enables the ELSTRN case control command to request elastic strain on elements or nodes, depending on the solution type.
Plate Curvature	Specifies the STRCUR or FIBER locations where elastic strain is output for shell elements.Note: SOL 402 ignores these options. The location of the output is based on the element type:For solid elements, the elastic strain is output at the corners.For shell elements, the elastic strain is output at the top and bottom of each element.For composite solid elements, the elastic strain is output at the top and bottom of each solid ply.For composite shell elements, the elastic strain is output at the midplane of each ply.
Location	Specifies the CENTER, CORNER, SGAGE, or CUBIC locations where elastic strain is output for CQUAD4 elements.Note: SOL 402 ignores these options. The location of the output is based on the element type:For solid element, the elastic strain is output at the corners.For shell elements, the elastic strain is output at the top and bottom of each element.For composite solid elements, the elastic strain is output at the top and bottom of each solid ply.For composite shell elements, the elastic strain is output at the midplane of each ply.SOL 402 does not support elastic strain for CBEAM, CROD, and CBAR elements.
Flexible Slider Result
Enable FLXRESULTS Request	Enables the FLXRESULTS case control command to request output from a flexible slider joint.
Curvilinear Abscissa	Outputs the relative displacement along the curvilinear abscissa for each selected sensor node. Each flexible slider can have one sensor node.
Entity	Lets you select the sensor nodes for which you want output.If you created your own sensor nodes, you can select the nodes for which you want output.If you let the solver create the sensor nodes, you can select output for all of the sensor nodes or none of them. You cannot select a subset of them.In the results, the node number for the sensors is used in the name of the XY curve generated by the solver.
Force
Enable FORCE Request	Enables the FORCE case control command to request element force or particle velocity output.
Location	Specifies the CENTER, CORNER, BILIN, or SGAGE options to control the location where element forces are output for CQUAD4 elements.For more information, see SGAGE, CUBIC, CORNER, BILIN Strain/Stress Options.
Gasket Result
Enable GKRESULTS Request	Enables the GKRESULTS case control command to request gasket results for SOLs 402 and 601 (SOL 601,106 Advanced Nonlinear Statics and SOL 601,129 Advanced Nonlinear Transient) analyses. Gasket results include gasket pressure, gasket closure, plastic gasket closure, gasket yield stress, and gasket status.
Glue Result
Enable BGRESULTS Request	Enables the BGRESULTS case control command to request grid point (node) force balance at selected grid points.
Pressure	Specifies the TRACTION option on the BGRESULTS case control command.
Force	Specifies the FORCE option on the BGRESULTS case control command.
Grid Point Force
Enable GPFORCE Request	Enables the GPFORCE case control command to request grid point (node) force balance at selected grid points.
Joint Result
Enable JRESULTS Request	Enables the JRESULTS case control command to request output from a kinematic joint.All of the outputs are in the coordinate system of the joint definition.
Force	Outputs the force vector.
Moment	Outputs the moment vector.
Displacement	Outputs the relative position between the kinematic joint nodes.
Angle	Outputs the relative rotation between the kinematic joint nodes.
Velocity	Outputs the relative velocity between the kinematic joint nodes.
Angular Velocity	Outputs the relative angular velocity between the kinematic joint nodes.
Entity	Lets you select the CJOINT elements for which you want output.
Kinetic Energy
Enable EKE Request	Enables the EKE case control command to request kinetic energy of selected elements.
Energy	Specifies the AVERAGE, AMPLITUDE, or PEAK options to control the type of energy results reported.
Threshold	Specifies the THRESH option. If you select THRESH, enter a Threshold value. The software suppresses kinetic energies for elements that have an energy value less than the defined threshold.
Modal Effective Mass
Enable MEFFMASS Request	Enables the MEFFMASS case control command to request output of modal effective mass, participation factors, and modal effective mass fractions in normal modes analyses.
Reference Grid Point	Specifies the GRID option, which lets you designate the reference grid point (node) to use to calculate the rigid body mass matrix. The default is the origin of the Absolute coordinate system.
Summary	Specifies the SUMMARY option to request the calculation of the total effective mass fraction, the modal effective mass matrix, and the rigid body mass matrix.
Modal Participation Factors	Specifies the PARTFAC option to request calculation of modal participation factors.
Modal Effective Mass	Specifies the MEFFM or MEFFW option to request calculation of modal effective mass.MEFFMRequests the calculation in units of mass.MEFFWRequests the calculation in units of weight.MEFFM, MEFFWRequests the calculation in units of mass and weight.
Modal Effective Mass Fraction	Specifies the FRACSUM option to request the calculation of the modal effective mass fraction.
MPC Forces
Enable MPCFORCES Request	Enables the MPCFORCES case control command to request multipoint force of constraint vector output.
Plastic Strain
Enable PLSTRN Request	Enables the PLSTRN case control command to request plastic strain output at nodes for SOLs 401 and 402.
Pressure
Enable OPRESS Request	Enables the OPRESS case control command to request the following output:Coupled PressureRequests output of the pressures computed by the flow solver in Simcenter 3D Multiphysics. Applies only to Multiphysics.Fluid Pressure PenetrationRequests output from the Fluid Penetration Pressure (PLOADFP) load.Applies to Multiphysics and SOLs 401 and 402.
Progressive Failure Results
Enable PFRESULTS Request	Enables the PFRESULTS case control command to request progressive failure results output for composite shell and solid elements for SOLs 401 and 402.
Nonlinear Stress
Enable NLSTRESS Request	Enables the NLSTRESS case control command to request the output of nonlinear element stresses for SOL 106 Nonlinear Statics analyses.
Shell Thickness
Enable SHELLTHK Request	Enables the SHELLTHK case control command to request the output of shell element thickness values for SOLs 402, 601, and 701 analyses.Note: Simcenter Nastran only outputs shell thickness results for large strain analyses (analyses in which you include the parameter PARAM, LGSTRN, 1). In Pre/Post, to set this parameter, select the Large Strains check box on the Parameters page of the Create Solution or Edit Solution dialog box.
SPC Forces
Enable SPCFORCES Request	Enables the SPCFORCES case control command to request single point force of constraint vector output.
Strain
Enable EKE Request	Enables the STRAIN case control command to request strain output.
Yield Criterion	Specifies the VONMISES or MAXS options to control the type of strain yield criterion.
Plate Curvature	Specifies the STRCUR or FIBER options to control the locations where strain is computed for plate elements.
Location	Specifies the CENTER, CORNER, BILIN, or SGAGE options to control the location where strain is output for CQUAD4 elements.
Composite Solid Ply Output	Controls the location of strain output for CHEXA and CPENTA type elements whose physical properties are defined with a Solid Laminate (PCOMPS) type of physical property.CPLYMIDRequests the stresses or strains at the middle of each ply.CPLYBTRequests the stresses or strains at the bottom and the top of each ply.CPLYBMTRequests the stresses or strains at the bottom, middle, and top of each ply.
Strain/Kinetic Energy Tabulation
Enable SEKETAB Request	Enables the SEKETAB case control command to compute the percentage of strain energy and the percentage of kinetic energy for specified groups of elements. The software writes the output to the .f06 file and to a .csv file, which you can open in a spreadsheet application.Note: If your solution contains multiple modes subcases, the .csv file includes energy output for only the last modes subcase. The .f06 file includes energy output tables for each modes subcase.In the Entity Selection group, you must select at least one group of elements or create a new group.
Strain Energy
Enable ESE Request	Enables the ESE case control command to request strain energy output for selected elements.
Energy	Specifies the AVERAGE, AMPLITUDE, or PEAK options to control the type of energy results reported.
Threshold	Specifies the THRESH option. If you select THRESH, enter a Threshold value. The software suppresses strain energies for elements that have an energy value less than the defined threshold.
Stress
Enable STRESS Request	Enables the STRESS case control command to request element stress output.
Yield Criterion	Specifies the VONMISES or MAXS options to control the type of stress yield criterion.
Location	Specifies the CENTER, CORNER, BILIN, or SGAGE options to control the location where stress is output for CQUAD4 elements.
Composite Solid Ply Output	Controls the location of stress output for CHEXA and CPENTA type elements whose physical properties are defined with a Solid Laminate (PCOMPS) type of physical property.CPLYMIDRequests the stresses or strains at the middle of each ply.CPLYBTRequests the stresses or strains at the bottom and the top of each ply.CPLYBMTRequests the stresses or strains at the bottom, middle, and top of each ply.
Thermal Strain
Enable THSTRN Request	Enables the THSTRN case control command to request velocity vector output.
Velocity
Enable VELOCITY Request	Enables the VELOCITY case control command to request velocity vector output.

FRF Output Requests options

Acceleration
Enable ACCELERATION Request	Specifies the ACCELERATION case control command to request acceleration over unit excitation load output.
Acoustic Pressure
Enable PRESSURE Request	Appears when Solution type is Acoustic or Vibro-Acoustic.Specifies the PRESSURE case control command to request pressure over unit excitation load output on fluid nodes or microphone nodes.
Displacement
Enable DISPLACEMENT Request	Specifies the DISPLACEMENT case control command to request displacement over unit excitation load output.
SPC Forces
Enable SPC Forces Request	Specifies the SPC Forces case control command to request force over unit excitation load output.Note: If the excitation is a Unit Force, SPCFORCES are not available and must be cleared.If the Enforced Motion excitation is used, SPCFORCES are valid and will be computed.
Velocity
Enable VELOCITY Request	Specifies the VELOCITY case control command to request velocity over unit excitation load output.
Frequencies
Frequencies	Specifies the forcing frequencies at which to output results.DefaultOutput results in accordance with the default behavior of the underlying Simcenter Nastran case control command.For example, if the underlying case control command is DISPLACEMENT, results are output at all forcing frequencies.ALLOutput results for all forcing frequencies.Specify FrequenciesOutput results for a subset of forcing frequencies that you specify.PEAKOUTOutput results for the subset of forcing frequencies that have the greatest response as determined by a PEAKOUT Criteria modeling object.For more information, see Limiting frequency response output to peak responses.

Thermal Output Requests options

Flux
Enable FLUX Request	Enables the FLUX case control command to request heat transfer gradient and flux output for heat transfer analyses.
Thermal
Enable THERMAL Request	Enables the THERMAL case control command to request temperature output.

Learn more

Requesting output for Nastran analyses

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Structural, FRF, and Thermal Output Requests dialog boxes (Nastran), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });