Structural Output Requests dialog box (Multiphysics)

Common options

Name and Description
Name	Defines the name of the modeling object.
Label	Specifies a unique numerical identifier for the modeling object.
Description	Enter a brief description or click to open a text editor where you can enter a longer description.
Preview Output Requests	Opens an information window where you can examine all current output requests and their options.
Enable All Output Requests	Selects all output requests.
Disable All Output Requests	Clears all output requests.
Common output request options
Sorting	Specifies SORT1 or SORT2 options to control the format of printed output.If you choose Default, the software chooses the default option for you analysis type. For example, SORT1 is the defautl in static analysis, while SORT2 is the default in transient response analysis.
Output Medium	Specifies PRINT, PUNCH, or PLOT options, depending on the case control command, to control the output destination for the results.If you select PRINT, the software outputs the results to the printer.If you select PUNCH, the software outputs the results to the .pch (ASCII format) file.If you select PLOT, the software reports the results in the OP2 file.See Simcenter Nastran Output Files in the Simcenter Nastran User's Guide for more information.
Data Format	Specifies REAL, IMAG, or PHASE options, depending on the case control command, to control the format of complex output.
Random Functions	Specifies PSDF, ATOC, or RALL options to request the calculation of specific random functions.
Entity Selection	Specifies ALL, NONE, or n (Set) options, depending on the case control command, to control the location at which the software outputs results. If you choose Set, select the appropriate node or element set.

Structural Output Requests options

Acceleration
Enable ACCELERATION Request	Specifies the ACCELERATION case control command to request acceleration vector output.
Adaptive Meshing
Enable ADAPTERR Request	Specifies the ADAPTERR case control command to control the computation and output of error estimates for adaptive meshing for Multiphysics solutions.
Stress Norm	Controls whether the software computes the stress norm and the stress error norm.Select STRESS to compute the stress and stress error norm values.Select None if you do not want to compute these values.
Strain Energy Norm	Controls whether the software computes the stress norm and the stress error norm.Select STNERGY to compute the strain and strain error norm values.Select None if you do not want to compute these values.
Individual Solution Time Results	Controls whether the software writes the specified error estimates at the output increment steps defined with the TSTEP1 entries.
Applied Load
Enable OLOAD Request	Specifies the OLOAD case control command to request applied load vector output.
Bolt Results
Enable BOLTRESULTS Request	Specifies the BOLTRESULTS case control command to request results for bolted connections.
Chocking Gap Distance
Enable CKGAP Request	Specifies the CKGAP case control command to calculate gap results for chocking elements.
Cohesive Element Results
Enable CZRESULTS Request	Specifies the CZRESULTS case control command to calculate results for cohesive elements.
Contact Result
Enable BCRESULTS Request	Specifies the BCRESULTS case control command to request contact results output for Simcenter Nastran SOL 601.
Pressure	Specifies the TRACTION option on the BCRESULTS case control command.
Creep Strain
Enable CRSTRN Request	Specifies the CRSTRN case control command to request the output of creep strain at nodes.
Displacement
Enable DISPLACEMENT Request	Specifies the DISPLACEMENT case control command to request displacement or pressure vector output.
Elastic Strain
Enable ELSTRN Request	Specifies the ELSTRN case control command to request the output of elastic strain at elements.
Force
Enable FORCE Request	Specifies 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.
Gauss Point Creep Strain
Enable GCRSTRN	Specifies the GCRSTRN case control command to request the output of creep strain at gauss points.
Gauss Point Elastic Strain
Enable GELSTRN Request	Specifies the GELSTRN case control command to request the output of elastic strain at gauss points.
Gauss Point Plastic Strain
Enable GPLSTRN Request	Specifies the GPLSTRN case control command to request the output of plastic strain at gauss points.
Gauss Point Strain
Enable GSTRAIN Request	Specifies the GSTRAIN case control command to request the output of strain at gauss points.
Gauss Point Stress
Enable GSTRESS Request	Specifies the GSTRESS case control command to request the output of stress at gauss points.
Gauss Point Thermal Strain
Enable GTHSTRN Request	Specifies the GTHSTRN case control command to request the output of thermal strain at gauss points.
Glue Result
Enable BGRESULTS Request	Specifies 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	Specifies the GPFORCE case control command to request grid point (node) force balance at selected grid points.
Kinetic Energy
Enable EKE Request	Specifies 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	Specifies 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 basic 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.Select MEFFM to request the calculation in units of mass.Select MEFFW to request the calculation in units of weight.Select MEFFM, MEFFW to request the calculation in units of mass and weight.
Modal Effective Mass	Specifies the FRACSUM option to request the calculation of the modal effective mass fraction.
Modal Effective Mass Fraction	Specifies the PARTFAC option to request calculation of modal participation factors.
MPC Forces
Enable MPCFORCES Request	Specifies the MPCFORCES case control command to request multipoint force of constraint vector output.
Plastic Strain
Enable PLSTRN Request	Specifies the PLSTRN case control command to request the output of plastic strain values at nodes.
Progressive Failure Results
Enable PFRESULTS Request	Specifies the PFRESULTS case control command to request of progressive failure results for composite solid elements.
Pressure
Enable OPRESS Request	Specifies the OPRESS case control command to request solution set pressure output.
SPC Forces
Enable SPCFORCES Request	Specifies the SPCFORCES case control command to request single point force of constraint vector output.
State Variable
Enable STATVAR Request	Specifies the STATVAR case control command to request the output of state variables used by a user material subroutine.
Strain
Enable EKE Request	Specifies 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 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.Select:CPLYMID to request the stresses or strains at the middle of each ply.CPLYBT to request the stresses or strains at the bottom and the top of each ply.CPLYBMT to request the stresses or strains at the bottom, middle, and top of each ply.
Strain Energy
Enable ESE Request	Specifies 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.
Initial Strain
Enable OSTNINI Request	Specifies the OSTNINI case control command to request initial strain output.
Stress
Enable STRESS Request	Specifies 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.Select:CPLYMID to request the stresses or strains at the middle of each ply.CPLYBT to request the stresses or strains at the bottom and the top of each ply.CPLYBMT to request the stresses or strains at the bottom, middle, and top of each ply.
Thermal Strain
Enable THSTRN Request	Specifies the THSTRN case control command to request the output of thermal strain values at nodes on elements.
Temperature
Enable OTEMP Request	Specifies the OTEMP case control command to request the output of temperature values on nodes.
Velocity
Enable VELOCITY Request	Specifies the VELOCITY case control command to request velocity vector output.

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Structural Output Requests dialog box (Multiphysics), 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 } });