Solution dialog box (Nastran), Case Control page

Option	Description	Corresponding Nastran syntax	Supported Nastran solutions
Title/Subtitle	Sets the title and/or subtitle for your solution.		All solutions
Flexible Body Solution Type	Specifies the type of solution to run.ExportWrites MBDEXPORT to export an input file for the multi-body dynamics software solve (Rflex .rfi input file for input to the RecurDyn solver, .mnf input file to the Adams solver, or .op2 file for the Simcenter 3D Motion Solver).RecoverWrites MBDRECVR to import the modal deformations file from multi-body dynamics software to perform results recovery.For more information, see the Multi-body Dynamics and Control System Software Interfaces chapter in the Simcenter Nastran Advanced Dynamic Analysis User's Guide.Note: If you will use the Simcenter 3D Motion application to run a flexible body analysis, you must leave this option set to Export.	MBDEXPORTMBDRECVR	SOL 103 Flexible Body
Flexible Body Export Options	Appears when Flexible Body Solution Type is set to Export.For descriptions of these options, see MBDEXPORT.Note: If you will use Simcenter 3D Motion to run a flexible body analysis, do not change any of these options.	MBDEXPORT	SOL 103 Flexible Body
Flexible Body Recovery Options	Appears when Flexible Body Solution Type is set to Recover.For descriptions of these options, see MBDRECVR.	MBDRECVR	SOL 103 Flexible Body
Number of Modal DOFs to be Retained	Sets the number of modal DOFs to retain.This value should be equal to or greater than the number of constrained normal modes. If this value is too low, some of the modes that you solve for will be ignored.For example, if you set the range of normal modes from 0 to 1200 Hz, then Nastran computes 650 modes. If Number of Modal DOFs to be Retained is set to 500, then the last 150 modes would be ignored for the flexible mode reduction. As a result, the flexible body results would still be valid, but they would be less accurate.After solving for the modes, Nastran removes any unneeded DOFs, so there is no risk in specifying a high number of DOFs to retain (such as 5000).	QSET, SPOINT	SOL 103 Flexible Body
Superelement Options	Lets you specify case control options for an external superelement solution.	EXTSEOUT	SOL 101 SuperelementSOL 103 Superelement
Bulk Data Echo Request	Controls the printout of bulk data.For more information, see Printing bulk data in your results file.	ECHO	All solutions
Rigid Body Checks	Specifies the motion grounding and mass reduction of rigid bodies in the solution.Select an existing modeling object from the list or click Create Modeling Object to create a new one.For more information, see Checking for unintentional grounding and mass reduction.	GROUNDCHECKWEIGHTCHECK	SOLs 101–112SOL 144 Static Aeroelastic ResponseSOL 145 Aeroelastic FlutterSOL 200 Design Sensitivity AnalysisSOL 200 Topology Optimization
Rigid Element Method	Specifies the rigid element processing method for RBAR, RBE1, RBE2, RBE3, and RROD elements.	RIGID	SOLs 101–112SOL 200 Design Sensitivity AnalysisSOL 200 Topology OptimizationSOL 401 Multi-Step Nonlinear (Simcenter Nastran)
Global Glue Parameters	Specifies the glue algorithm for following conditions:Edge-to-edge glueEdge-to-surface glueSurface-to-surface glueFor more information, see Glue Control ParametersFor more information about Glue Parameters dialog box, see Glue Parameters–Linear Global dialog box (Simcenter Nastran)	BGPARM	SOL 108 Direct Frequency Response FunctionsSOL 108 Vibro-Acoustic Transfer VectorSOL 111 Modal Frequency Response FunctionsSOL 111 Vibro-Acoustic Transfer Vector
Fluid-Structure Interaction Control Parameters	Specifies the fluid-structure interaction control parameters required for defining coupling.For more information, see Fluid-structure interaction control.For more information about Fluid-Structure Interaction Control Parameters dialog box, see Fluid-Structure Interaction Control Parameters dialog box (Nastran).	FLSTCNT	SOL 103 Real Eigenvalues (Vibro-Acoustic)SOL 107 Direct Complex Eigenvalues (Vibro-Acoustic)SOL 108 Direct Frequency Response Functions (Vibro-Acoustic)SOL 108 Vibro-Acoustic Transfer Vector (Vibro-Acoustic)SOL 111 Modal Frequency Response Functions (Vibro-Acoustic)SOL 111 Vibro-Acoustic Transfer Vector (Vibro-Acoustic)SOL 200 Design Sensitivity Analysis (Vibro-Acoustic)
Output Requests	Specifies the output request for the solution.Select an existing modeling object from the list or click Create Modeling Object to create a new one.Click Edit to edit the selected modeling object.See Requesting output for Nastran analyses.		All solutions except SOL 103 Response Dynamics
Vibro-Acoustic Transfer Vector Response Output Requests	Specifies the output request for the solution.Select an existing modeling object from the list or click Create Modeling Object to create a new one.Click Edit to edit the selected modeling object.See Requesting output for Nastran analyses.		SOL 108 Vibro-Acoustic Transfer Vector Response
Design Sensitivity Output	Specifies the design sensitivity output parameters.With Headings and LabelsPrints the output with headings and labels.Matrix PrintPrints the output as general matrix data blocks.For more information, see MATPRN.No OutputPrints no output.	DSAPRT	SOL 200 Design Sensitivity Analysis
Forcing Frequencies	Specifies forcing frequencies for use during a structural, acoustic, or a vibro-acoustic analysis.Click Create Forcing Frequencies to create a new Forcing Frequencies or Forcing Frequencies - Modal modeling object.Click Edit Forcing Frequencies to edit the selected modeling object.	FREQ, FREQ1, or FREQ2	Forcing Frequencies modeling object:SOL 108 Acoustic Transfer VectorSOL 108 Direct Frequency ResponseSOL 111 Modal Frequency ResponseSOL 200 Design Sensitivity Analysis
FREQ3, FREQ4, or FREQ5	Forcing Frequencies - Modal modeling object:SOL 111 Modal Frequency Response
Global Contact Parameters	In Simcenter Nastran solutions, when you include a Surface-to-Surface Contact simulation object in your solution, lets you select a Contact Parameters - Linear global modeling object to adjust contact parameters.For more information, see Defining parameters for contact conditions (Simcenter Nastran).In MSC Nastran solutions, when you include a General Contact/Glue simulation object in your solution, lets you select a Global Geometric Contact Parameters modeling object to adjust contact parameters.For more information, see Contact and glue conditions for MSC Nastran.	BCTPARM (Simcenter Nastran)BCPARA (MSC Nastran)	SOL 101 Global ConstraintsSOL 101 Subcase ConstraintsSOL 103 Real Eigenvalues (MSC Nastran)SOL 200 Design Sensitivity AnalysisSOL 200 Topology Optimization (Simcenter Nastran)SOL 401 Multi-Step Nonlinear (Simcenter Nastran)
Global Glue Parameters	When you include a Surface-to-Surface Gluing simulation object in your solution, lets you select a Glue Parameters modeling object to the adjust Simcenter Nastran glue algorithm.For more information, see Defining parameters for glue conditions.	BGPARM	All solutions except the following:SOL 144 Static Aeroelastic ResponseSOL 145 Aeroelastic FlutterSOL 200 Design Sensitivity Analysis (MSC Nastran)SOL 414 analysesSOL 701 Explicit Advanced Nonlinear Analysis
Design Objective	The overall single goal of the optimization problem. With the Design Objective, you choose whether to minimize or maximize a particular design response. The objective references a design response that is defined in a Design Response Quantities modeling object.	DESOBJ	SOL 200 Design Optimization
Design Constraints	The upper and lower bounds on the design responses. Each Design Constraint references a design response that is defined in a Design Response Quantities modeling object.	DCONSTR	SOL 200 Design Optimization
Fourier Harmonics	Requests the harmonic numbers of harmonic behavior for Fourier elements.	FHAR	SOL 402 Multi-Step Nonlinear KinematicsAll SOL 414 solution types
Fourier Harmonics to Constrain	Removes Fourier harmonic numbers.	FHAC	SOL 402 Multi-Step Nonlinear KinematicsAll SOL 414 solution types
Cyclic Symmetry Waves	Requests the solution harmonics for cyclic symmetry.	HARMONICS	SOL 414,103 Eigenvalues and Superelement ReductionSOL 414,110 Complex Modal Analysis
Nonlinear Parameters or Global Nonlinear Control Parameters or Nonlinear Control Parameters	Specifies a modeling object to define parameters that control the iteration strategy for the analysis. See Controlling the iteration strategy in Nastran nonlinear analyses for more information.	NLPARM (SOL 106 and SOL 153)NLCNTL (SOL 401)NLCNTLG (SOL 401, SOL 402, SOL 414)NLCNTL2 (SOL 402, SOL 414,129; SOL 414,103 for Transient Preload subcase)	SOL 106 Nonlinear StaticsSOL 153 Steady State Nonlinear Heat TransferSOL 401 Multi-Step NonlinearSOL 402 Multi-Step Nonlinear KinematicsSOL 414
Virtual Thread Parameters	Specifies a modeling object to define parameters that control contact for bolts modeled with the Virtual Thread Contact simulation object. For more information, see Modeling bolt threads (SOL 402).	BVTPAR	SOL 402 Multi-Step Nonlinear Kinematics
Arc-Length Methods Parameters	Controls the arc-length incremental solution strategies in nonlinear static analysis (SOL 106).	NLPCI	SOL 106 Nonlinear Statics
Real Eigenvalue Method for Structure	Specifies the modeling object that controls the eigenvalue extraction method to use for the structural portion of the model.You can use either the Lanczos or Householder method.Select an existing modeling object from the list or click Open Manager to create a new Real Eigenvalue - Lanczos or Real Eigenvalue - Householder modeling object.Click Edit to edit the selected modeling object.	METHOD	SOL 103 Real Eigenvalues (Vibro-Acoustic)SOL 110 Modal Complex Eigenvalues (Vibro-Acoustic)SOL 111 Modal Frequency Response (Vibro-Acoustic)SOL 200 Design Sensitivity Analysis (Vibro-Acoustic)
Real Eigenvalue Method for Fluid	Specifies the modeling object that controls the eigenvalue extraction method to use for the fluid portion of the model.You can use either the Lanczos or Householder method.Select an existing modeling object from the list or click Open Manager to create a new Real Eigenvalue - Lanczos or Real Eigenvalue - Householder modeling object.Click Edit to edit the selected modeling object.	METHOD	SOL 103 Real Eigenvalues (Vibro-Acoustic)SOL 110 Modal Complex Eigenvalues (Vibro-Acoustic)SOL 111 Modal Frequency Response (Vibro-Acoustic)SOL 200 Design Sensitivity Analysis (Vibro-Acoustic)
Real Eigenvalue Extraction Data/Method****Eigenvalue Method	Specifies Lanczos or Householder as the eigenvalue extraction method.	METHOD	SOL 103 Real Eigenvalues (Structural)SOL 110 Modal Complex EigenvaluesSOL 111 Modal Frequency ResponseSOL 112 Modal Transient ResponseSOL 145 Aeroelastic FlutterSOL 200 Design Sensitivity Analysis (Structural)
Lanczos MethodLanczos DataHouseholder Method****Householder Data	Specifies the real eigenvalue extraction options for the solution. Eigenvalue extraction options are stored as a solver-specific modeling object.Select an existing modeling object from the list or click Create Modeling Object to create a new one.Click Edit to edit the selected modeling object.For more information, see Defining eigenvalue extraction data for Nastran analyses.	EIGRL or EIGR	SOL 103 Real EigenvaluesSOL 111 Modal Frequency ResponseSOL 112 Modal Transient ResponseSOL 145 Aeroelastic FlutterSOL 200 Design Sensitivity Analysis (Structural)
Recursive Domain Normal ModesRecursive Domain Normal Modes for StructureRecursive Domain Normal Modes for Fluid	For a structural analysis, appear when Eigenvalue Method is set to Lanczos.Specifies the modeling object that partitions large scale normal modes analysis into subdomains.Note: For a vibro-acoustic analysis, the structural RDMODES bulk data entry is exported only when you have specified a Real Eigenvalue - Lanczos modeling object for Real Eigenvalue Method for Structure.For an acoustic or vibro-acoustic analysis, the fluid RDMODES bulk data entry is exported only when you have specified a Real Eigenvalue - Lanczos modeling object for Real Eigenvalue Method for Fluid.	RDMODES	SOL 103 Real EigenvaluesSOL 111 Modal Frequency Response
Residual Vectors	Specifies the modeling object that controls the output of residual vectors.Select an existing modeling object from the list or click Create Modeling Object to create a new one.Click Edit to edit the selected modeling object.For more information, see Modal truncation effects.	RESVEC	Structural as the specified analysis type: SOL 103 Flexible BodySOL 103 SuperelementSOL 112 Modal Transient ResponseStructural as the specified analysis type and Subcase - Dynamics as the solution step:SOL 103 Response DynamicsStructural or Vibro-Acoustic as the specified analysis type:SOL 103 Real EigenvaluesSOL 110 Modal Complex EigenvaluesSOL 111 Modal Frequency ResponseSOL 200 Design Sensitivity Analysis
Mode SelectionNote: For a vibro-acoustic analysis, you can use Mode Selection for Structure and Mode Selection for Fluid to specify separate mode selections for the structure and fluid.	Specifies the mode numbers of the structural or fluid modes to consider for the response computation (perhaps after you have solved the solution and you know the mode numbers that were computed).You can include all modes, or specify specific modes to include or exclude.Select an existing modeling object from the list or click Create Modeling Object to create a new one.Click Edit to edit the selected modeling object.	MODSEL (Simcenter Nastran)MODESELECT (MSC Nastran)	SOL 103 Real EigenvaluesSOL 110 Modal Complex EigenvaluesSOL 111 Modal Frequency ResponseSOL 145 Aeroelastic FlutterSOL 200 Design Sensitivity Analysis
Modal DampingNote: For a vibro-acoustic analysis, you can specify separate structural and fluid modal damping values. These options appear under the Modal Damping for Structure and Modal Damping for Fluid groups.	Defines the type of damping units (for structure and fluid) to use for the modal damping values (gi, etc.).StructuralDamping values are in units of equivalent viscous dampers.CriticalDamping values are in units of fraction of critical damping C/C0.Amplification FactorDamping values are in units of the amplification of quality factor, Q.This option corresponds to the Nastran SDAMPING bulk entry.	SDAMPING	SOL 111 Modal Frequency ResponseSOL 200 Design Sensitivity Analysis
Structural Damping / Critical Damping / Amplification Factor Damping	Specifies the modal damping value.For more information, see Additional magnitude options.	TABDMP1	SOL 111 Modal Frequency ResponseSOL 111 Modal Frequency Response FunctionsSOL 111 Vibro-Acoustic Transfer VectorSOL 200 Design Sensitivity Analysis (DSA - Modal Frequency and DSA - Modal Frequency Response Functions)SOL 200 Topology Optimization (Nastopt - Modal Frequency)
Time Step Intervals	Specifies the time steps for the solution.Select an existing modeling object from the list or click Create Modeling Object to create a new one.Click Edit to edit the selected modeling object.See Defining time step intervals for transient or nonlinear analyses.	TSTEP	SOL 601,106 Advanced Nonlinear StaticsSOL 601,129 Advanced Nonlinear TransientSOL 701 Explicit Advanced Nonlinear Analysis
PEAKOUT Criteria	Specifies PEAKOUT Criteria for use during a structural or vibro-acoustic analysis.Click Create PEAKOUT Criteria to define new criteria parameters for automatic identification of loading frequencies at which result peaks occur.Click Edit PEAKOUT Criteria to edit the selected modeling object.For more information, see PEAKOUT Criteria dialog box.	PEAKOUT	SOL 108 Direct Frequency Response SOL 108 Vibro-Acoustic Transfer Vector ResponseSOL 111 Modal Frequency Response
Range of Forcing Frequencies (FREQV)	Specifies frequency range of interest for a vibro-acoustic transfer vector (VATV) response analysis. The exact frequencies are derived from the VATV matrix computed frequencies in the specified frequency range.Click Enable Frequency Range to enter a Minimum Frequency and Maximum Frequency.Note: If you do not specify any values for Minimum Frequency and Maximum Frequency, the software will use all derived VATV matrix computed frequencies.	FREQV	SOL 108 Vibro-Acoustic Transfer Vector Response
Parameters (PARAM)	Specifies the parameters to include in the case control section of your input file.Select an existing modeling object from the list or click Create Modeling Object to create a new one.Click Edit to edit the selected modeling object.Use the options in the Solution Parameters dialog box to specify the options for the PARAM bulk data entry.For more information, see Specifying parameters for Nastran analyses.	Parameter Descriptions	All solutions except the following:SOL 402 Multi-Step Nonlinear KinematicsAll SOL 414 solutions
User Defined Text	Specifies the comments or file to include in the File Management section of your Nastran input file.Select an existing modeling object from the list or click Create Modeling Object to create a new one.Click Edit to edit the selected modeling object.For more information, see Customizing a Nastran input file with user defined text	$ or INCLUDE	All solutions
Monitor Point Type to Output	Controls the printout of monitor point data to the .f06 file.DefaultDoes not write the MONITOR case control command to the Simcenter Nastran case control section, and does not request the output of monitor data. This option is useful when you do not want the command to be exported to the Simcenter Nastran .dat file.ALLRequests the output of monitor point data.NONEDoes not output monitor point data, but does write the MONITOR case control command to the Simcenter Nastran .dat file case control section.	MONITOR (Simcenter Nastran)	SOL 101 Linear Statics - Global Constraints (Structural and Axisymmetric Structural analyses)SOL 101 Linear Statics - Subcase Constraints (Structural and Axisymmetric Structural analyses)SOL 103 Real Eigenvalues (structural and vibro-acoustic analyses)
Monitor Points to Exclude	Appears when Monitor Point Type to Output is set to ALL.Lets you control the exclusion of monitor point types.NoneDoes not exclude any monitor point types.MONPNT2Excludes MONPNT2 types.MONPNT3Excludes MONPNT3 types.	MONITOR (Simcenter Nastran)	SOL 101 Linear Statics - Global Constraints (structural and axisymmetric structural analyses)SOL 101 Linear Statics - Subcase Constraints (structural and axisymmetric structural analyses)SOL 103 Real Eigenvalues (structural and vibro-acoustic analyses)
Aerodynamic Symmetry XY	Lets you specify symmetry with respect to the XY-plane in an aeroelastic model.SymmetricIn the XY-plane of the model, displacement in the Z-direction is zero and rotation about the X-axis and Y-axis are zero.AntisymmetricIn the XY-plane of the model, displacement in the X-direction and Y-direction are zero and rotation about the Z-axis is zero.**Asymmetric (No Reflection)**The XY-plane is not a plane of symmetry.		SOL 144 Static Aeroelastic ResponseSOL 145 Aeroelastic Flutter
Aerodynamic Symmetry XZ	Lets you specify symmetry with respect to the XZ-plane in an aeroelastic model.SymmetricIn the XZ-plane of the model, displacement in the Y-direction is zero and rotation about the X-axis and Z-axis are zero.AntisymmetricIn the XZ-plane of the model, displacement in the X-direction and Z-direction are zero and rotation about the Y-axis is zero.**Asymmetric (No Reflection)**The XZ-plane is not a plane of symmetry.		SOL 144 Static Aeroelastic ResponseSOL 145 Aeroelastic Flutter
Flutter Data	Lets you specify the flutter analysis method and related data.	FLUTTER	SOL 145 Aeroelastic Flutter
Structural Damping	Lets you specify hysteretic damping in a flutter analysis.		SOL 145 Aeroelastic Flutter
Rotor Dynamics
Available for non-SOL 414 rotor dynamics solutions.
Complex Mode Reduction	Specifies the complex mode reduction for use during a direct complex eigenvalue rotor dynamic analysis or a vibro-acoustic analysis.Select an existing modeling object from the list or click Create Modeling Object to create a new one.Click Edit to edit the selected modeling object.	RMETHOD or EIGC	SOL 107 Direct Complex EigenvaluesSOL 110 Modal Complex Eigenvalues

How do I

Create or modify a solution

Create or modify a solution step or subcase

Learn more

Solutions

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Solution dialog box (Nastran), Case Control page, 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 } });