Multiphysics

Requesting structural output for Simcenter 3D Multiphysics

You use a Structural Output Requests modeling object to request the types of structural output the software lists to the F06, OP2, or PUNCH (.pch) file when you solve your structural analysis or the structural portion of a coupled analysis in a Simcenter 3D Multiphysics solution. When you create an output request, you select each type of result you want the solver to output. Each individual output type corresponds to a Simcenter Nastran case control command. When you enable an output request, the software creates the corresponding case control entry in the case control section of your input file. For example, if you want the software to output applied loads, select the Enable OLOAD Request option.

Types of output available

The tabbed pages on the Structural Output Requests dialog box let you select specific output types as well as options to control each output type. For more information on the dialog box options, see Structural Output Requests dialog box (Multiphysics).

Output request type	Corresponding Nastran case control command	Description
Adaptive Meshing	ADAPTERR	Controls the computation and output of error estimates for adaptive meshing for Multiphysics solutions.For more information, see Adaptive meshing.
Applied Load	OLOAD	Requests applied load vector output.
Bolt Results	BOLTRESULTS	Requests bolt results.For more information, see Bolt pre-loads with Simcenter Nastran and Simcenter 3D Multiphysics.
Chocking Gap Distance	CKGAP	Requests gap results for chocking elements.For more information, see Chocking elements.
Cohesive Element Results	CZRESULTS	Requests results for cohesive elements.For more information, see Cohesive elements.
Contact Result	BCRESULTS	Requests contact results.
Creep Strain	CRSTRN	Requests the output of creep strain at nodes.
Cyclic Forces	CYCFORCES	Requests MPC force output at the nodes selected for the automatic coupling in a cyclic symmetry analysis.For more information, see Cyclic symmetric normal modes solutions.
Displacement	DISPLACEMENT	Requests displacement or pressure vector output.
Elastic Strain	ELSTRN	Requests the output of elastic strain at elements.
Force	FORCE	Requests element force output or particle velocity output in coupled fluid-structural analyses.
Gauss Point Creep Strain	GCRSTRN	Requests the output of creep strain at gauss points.
Gauss Point Elastic Strain	GELSTRN	Requests the output of elastic strain at gauss points.
Gauss Point Plastic Strain	GPLSTRN	Requests the output of plastic strain at gauss points.
Gauss Point Strain	GSTRAIN	Requests the output of strain at gauss points.
Gauss Point Stress	GSTRESS	Requests the output of stress at gauss points.
Gauss Point Thermal	GTHSTRN	Requests the output of thermal strain at gauss points.
Glue Result	BGRESULTS	Requests the output of glue results. The software calculates and stores glue tractions at the nodes that are located on the glued surfaces. The glue tractions, which are similar to contact results, are calculated and stored at the nodes that are located on the glue surfaces. The normal component of the tractions is a scalar value while the in-plane (tangential) tractions are output in the basic coordinate system.Note: For surfaces on which you have created an Edge-to-Surface Gluing definition, the software recovers only point forces and not surface tractions.
Grid Point Force	GPFORCE	Requests grid point (node) forces at selected grid point locations.
Initial Strain	OSTNINI	Requests initial strain output.
Kinetic Energy	EKE	Requests kinetic energy output for selected elements.
Modal Effective Mass	MEFFMASS	Requests output of modal effective mass, modal participation factors, and modal effective mass fractions in normal modes analyses.
MPC Forces	MPCFORCES	Requests multipoint force of constraint vector output.
Plastic Strain	PLSTRN	Requests the output of plastic strain values at nodes.
Pressure	OPRESS	Requests the solution set pressure output.
SPC Forces	SPCFORCES	Requests single point force of constraint vector output.
Strain	STRAIN	Requests strain output.
Strain Energy	ESE	Requests strain energy output for selected elements.
State Variable	STATVAR	Requests output of state variables used by a user defined material.For more information, see Simcenter Nastran user-defined material models.
Stress	STRESS	Requests stress output.
Thermal Strain	THSTRN	Requests the output of thermal strain values at nodes on elements.
Temperature	OTEMP	Requests the output of temperature values on nodes.

Customer defaults settings to control output request defaults

Customer Defaults options let you to control which output requests are selected by default in the Structural Output Requests dialog box. For example, if you are always interested in the displacement and stress results of your model in structural analyses, you can select Displacement and Stress in the Nastran Solution defaults. When you create a new Structural Output Request, those types of output are selected by default.

Where do I find it?

Application	Pre/Post
Prerequisite	An active Simulation file with Simcenter 3D Multiphysics as the specified solverStructural, Coupled Thermal-Structural, Coupled Flow-Structural, or Coupled Thermal-Flow-Structural as the specified Analysis Type
Command Finder	Modeling Objects →Type list→Structural Output Requests
Menu	Insert→Modeling Objects→Type list→Structural Output Requests

How do I

Define coupled solution parameters

Learn more

Simcenter 3D Multiphysics overview

Mapping results data to another model in Simcenter 3D Multiphysics

Two-way fluid-structure interaction

Defining multiphysics solution steps

Controlling time steps in a coupled solution

Requesting thermal, flow, and thermal-flow output for Simcenter 3D Multiphysics

Adding time points to a structural solution to match a reference solution

Previewing Multiphysics solver syntax

Analyzing multiphysics results

Controlling the export of nodes connected to flow elements

Look up more details

Simcenter 3D Multiphysics boundary conditions

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area