Solution Step/Subcase dialog box (Nastran)

Solution
Name	Sets the name of the subcase.
Solver Type	Displays the solver for the solution, such as Simcenter Nastran.
Analysis Type	Displays the analysis type, such as Structural or Vibro-acoustic.
Solution	Displays the solution type.
Step	Specifies the type of subcase to create.For some combinations of solver, analysis type, and solution type, you cannot change the subcase type.
Create Step	Appears when you create a new subcase.Displays the subcase options associated with the specified solver, analysis type, solution type, and subcase type.
Steps to Create	For certain solution types, appears when you add a subcase to an existing solution.Sets the number of subcases to create for this solution.
Relative Position	For certain solution types, appears when you add a subcase to an existing solution.Specifies the position where this subcase or subcases will be created in the solution relative to any existing subcases.

Option	Description	Supported Nastran solutions
Description	Sets a description for the solution step/subcase.You can also click Description to open the Description dialog box. This lets you see more of the text that you type, as well as cut, copy, or paste text.	All solutions
Use Step Name as Label	Controls whether the software uses the specified name as the label for the corresponding Nastran subcase.When you export or solve your model, the software uses the specified name to write out a LABEL case control command for the associated SUBCASE case control command in the Nastran input file.If you clear this check box, type the label to use in the Label box.If this check box does not appear, the exporter automatically creates a SUBCASE case control commands for each unit force or unit enforced motion degrees of freedom (DOFs) specified as loads. The LABEL case control command for each SUBCASE indicates the type of load, the node number, and the DOF being excited (for example, LOAD:NODE 2:+DOF6).	All solutions except for the following:SOL108 Direct Frequency Response (Subcase - Direct Frequency Response Functions)SOL111 Modal Frequency Response FunctionsSOL 200 Design Sensitivity Analysis (DSA - Modal Frequency Response Functions)
Label	Available when the Use Step Name as Label check box is cleared.Sets the name to use to write out a LABEL case control command for the associated SUBCASE case control command in the Nastran input file.	All solutions
Random Results Sorting	Appears when Step is set to Subcase – Random Distributed Acoustic Plane Waves.Specifies the format for the random analysis results.SORT1 (vector)SORT2 (function)	SOL108 Direct Frequency ResponseSOL111 Modal Frequency Response
Output Requests	Specifies the output request for the step or subcase.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.	All solutions except the following:SOL 108 Vibro-Acoustic Transfer VectorSOL 111 Vibro-Acoustic Transfer VectorSOL 108 Vibro-Acoustic Transfer Vector Response
Vibro-Acoustic Transfer Vector Output Request	Specifies the output request for the step or subcase.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.	SOL 108 Vibro-Acoustic Transfer VectorSOL 111 Vibro-Acoustic Transfer Vector
Vibro-Acoustic Transfer Vector Response Output Requests	Specifies the output request for the step or subcase.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.	SOL 108 Vibro-Acoustic Transfer Vector Response
Sequential Dependency on Previous Subcase	Specifies whether to make this subcase dependent on the end state (displacement, stress, and strain) of the previous subcase.To use the end state of the previous subcase as the initial state of this subcase, select Yes.If you restart this subcase with the Restart Computation Flag (RSUB) parameter for the nonlinear control parameters modeling object, the initial state is the same as the state at the end of the previous subcase.To start with a new state, select No.If you restart this subcase with the Restart Computation Flag (RSUB), the initial state is the same as the state at the initial computation time. Note: For dynamic and static subcases, the start time is always the end time of the previous time-based subcase, regardless of what you select.For more information on restarting a subcase, see Restart Options page.	SOL 401 Multi-Step Nonlinear (except Preload subcase)SOL 402 Multi-Step Nonlinear Kinematics (except Preload subcase)
Eigenvalue Method	Specifies the eigenvalue extraction method to use.See Eigenvalue Extraction Methods for a discussion of method selection.	SOL 103 Response Dynamics (Subcase - Dynamics)SOL 106 Nonlinear StaticsSOL 110 Modal Complex EigenvaluesSOL 111 Modal Frequency ResponseSOL 111 Modal Frequency Response FunctionsSOL 112 Modal Transient ResponseSOL 145 Aeroelastic FlutterSOL 200 Design Sensitivity Analysis (structural analysis)SOL 200 Topology Optimization (Nastopt - Normal Modes, Nastopt - Modal Frequency)SOL 401 Multi-Step Nonlinear (Normal Modes, Cyclic Modes)SOL 402 Multi-Step Nonlinear Kinematics (Normal Modes, Buckling, Cyclic Modes)
Lanczos Data****Householder Data	Specifies the real or complex eigenvalue extraction options for the step or subcase.These options correspond to the Nastran EIGRL, EIGR or EIGC bulk entries.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.	SOL 103 Response Dynamics (Subcase - Dynamics)SOL 110 Modal Complex EigenvaluesSOL 111 Modal Frequency ResponseSOL 112 Modal Transient ResponseSOL 145 Aeroelastic FlutterSOL 200 Design Sensitivity Analysis (structural analysis)SOL 200 Topology Optimization (Nastopt - Normal Modes, Nastopt - Modal Frequency)
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.This option corresponds to the Nastran RESVEC case control command.	Structural as the specified analysis type: SOL 103 Flexible BodySOL 103 SuperelementSOL 112 Modal Transient Response Structural as the specified analysis type and Subcase - Dynamics as the solution step:SOL 103 Response Dynamics Structural or Vibro-Acoustic as the specified analysis type:SOL 103 Real EigenvaluesSOL 110 Modal Complex EigenvaluesSOL 111 Modal Frequency ResponseSOL 111 Vibro-Acoustic Transfer VectorSOL 200 Design Sensitivity Analysis
Extraction Approach	Appears when Step is set to Subcase - Complex Modes.Specifies how you want the complex modes to be extracted.Modal ApproachLets you create a Real Eigenvalue - Lanczos or Complex Eigenvalue modeling object.Direct ApproachLets you create a Complex Eigenvalue modeling object.	SOL 402 Multi-Step Nonlinear Kinematics
Real Eigenvalue Method	Appears when Extraction Approach is set to Modal Approach.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.This option corresponds to the Nastran EIGRL case control command.	SOL 402 Multi-Step Nonlinear Kinematics
Complex Eigenvalue Method	This option corresponds to the Nastran EIGC case control command.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.	SOL 144 Static Aeroelastic Response (aeroelastic divergence analysis)SOL 402 Multi-Step Nonlinear Kinematics
Real Eigenvalue Method for Structure	This option corresponds to the Simcenter Nastran METHOD case control command and EIGRL bulk entry.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.	SOL 111 Vibro-Acoustic Transfer VectorSOL111 Modal Frequency ResponseSOL 200 Design Sensitivity Analysis (vibro-acoustic analysis)
Recursive Domain Normal Modes****Recursive Domain Normal Modes for Structure	For a structural analysis, appears when Eigenvalue Method is set to Lanczos.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.This option corresponds to the Simcenter Nastran RDMODES bulk entry.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. The fluid RDMODES bulk data entry is exported only when you have specified a Real Eigenvalue - Lanczos modeling object for the Real Eigenvalue Method for Fluid.	SOL111 Modal Frequency Response
Real Eigenvalue Method for Fluid	This option corresponds to the Simcenter Nastran METHOD case control command and EIGRL bulk entry.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.	SOL111 Modal Frequency ResponseSOL 200 Design Sensitivity Analysis (vibro-acoustic analysis)
Recursive Domain Normal Modes for Fluid	This option corresponds to the Simcenter Nastran RDMODES bulk entry.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.	SOL111 Modal Frequency Response
Mode Selection for Structure****Mode Selection for Fluid	This option corresponds to the Simcenter Nastran MODSEL case control command.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.	SOL 111 Vibro-Acoustic Transfer VectorSOL 200 Design Sensitivity Analysis (vibro-acoustic analysis, DSA - Modal Frequency and DSA - Modal Frequency Response Functions)
Nonlinear Control Parameters	Defines parameters that control the iteration strategy.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.This option corresponds to the Nastran NLCNTL bulk entry for SOL 401 and to the Nastran NLCNTL2 bulk entry for SOL 402.	SOL 401 Multi-Step NonlinearSOL 402 Multi-Step Nonlinear Kinematics
Trim Variables Constraint	Specifies the Trim Variables Constraint 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.	SOL 144 Static Aeroelastic Response (static aeroelastic analysis)
Variables Links	Specifies the Aerodynamic Variables Link modeling object.	SOL 144 Static Aeroelastic Response (static aeroelastic analysis)
Aerodynamic Divergence Data	Specifies the Aerodynamic Divergence Data 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.	SOL 144 Static Aeroelastic Response (aeroelastic divergence analysis)
Flutter Data	Specifies the flutter analysis method and related data.	SOL 145 Aeroelastic Flutter
Structural Damping	Specifies hysteretic damping in a flutter analysis.	SOL 145 Aeroelastic Flutter
Case Control Parameters (PARAM)	Specifies a Solution Parameters modeling object to include parameters in the case control section of your input file.Note: To specify the options for the PARAM bulk entry, use the options in the Solution Parameters dialog box.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 Specifying parameters for Nastran analyses.For information on setting the OIBULK parameter to include an unsorted copy of bulk entries in the Simcenter Nastran .op2 file, see Preserving the order and format of bulk data through the round-trip process.Note: Use the PARAM,OIBULK,YES parameter to import monitor point data from a Simcenter Nastran .op2 file.	All solutions except the following:SOL 402 Multi-Step Nonlinear KinematicsSOL 601,106 Advanced Nonlinear StaticsSOL 601,129 Advanced Nonlinear TransientSOL 701 Explicit Advanced Nonlinear AnalysisFor these solutions, you set the parameters on the Parameters page in the Solution dialog box.
Monitor Point Type to Output	Controls the printout of monitor point data to the .f06 file for the subcase.DefaultInherits the Monitor Point Type to Output setting on the Case Control page in the Solution dialog box.Does not write the MONITOR case control command to the subcase in the Simcenter Nastran .dat file case control section. ALLRequests the output of monitor point data.NONEDoes not output monitor point data. This option overrides the Monitor Point Type to Output setting in the Solution dialog box.This option corresponds to the Simcenter Nastran MONITOR case control command.	Structural or Axisymmetric Structural as the specified analysis type: SOL 101 Linear Statics - Global ConstraintsSOL 101 Linear Statics - Subcase ConstraintsStructural or Vibro-Acoustic as the specified analysis type:SOL 103 Real Eigenvalues
Monitor Points to Exclude	Appears when Monitor Point Type to Output is set to ALL.Lets you control the exclusion of monitor point types for the subcase.NoneDoes not exclude any monitor point types.MONPNT2Excludes MONPNT2 types.MONPNT3Excludes MONPNT3 types.This option corresponds to the Simcenter Nastran MONITOR case control command.	Structural or Axisymmetric Structural as the specified analysis type: SOL 101 Linear Statics - Global ConstraintsSOL 101 Linear Statics - Subcase ConstraintsStructural or Vibro-Acoustic as the specified analysis type:SOL 103 Real Eigenvalues
Case Control User Defined Text	Specifies the text to include in the 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.	All solutions
Random Analysis
Appears when Step is set to Subcase – Random.
Results Sorting	Specifies the format for the random analysis results.**Function Plot (SORT2)**Lets you visualize results in different function plots (XY plot, color map, color bars, waterfall, bar chart display, and so on).**Contour Plot (SORT1)**Lets you visualize results with a continuous range of colors that indicate the value of the plotted results.	Structural, Acoustic, or Vibro-Acoustic as the specified analysis type: SOL108 Direct Frequency ResponseSOL108 Vibro-Acoustic Transfer Vector ResponseSOL111 Modal Frequency Response
Power Spectral Density Factors Definition	Controls the definition of the power spectral density (PSD) factors. Power spectral definitions are stored as solver-specific modeling objects or in an HDF5 file.User DefinedLets you create a Power Spectral Density Factors modeling object.From FileLets you locate an HDF5 file. The software exports the file information to the Simcenter Nastran RANDPEX bulk entry.Note: This option makes it easier for you to recombine load cases after a PSD decomposition or time segmentation.
Frequency / PSD Data Interpolation	Appears when Power Spectral Density Factors Definition is set to From File.Lets you select the interpolation type for frequency abscissa and PSD data ordinate. The software exports the interpolation type to the Simcenter Nastran RANDPEX bulk entry.
Power Spectral Density Factors	Appears when Power Spectral Density Factors Definition is set to User Defined.Defines the power spectral density factors for the step or subcase. Power spectral definitions are stored as solver-specific modeling objects. The Power Spectral Density Factors modeling object provides the input for this random analysis subcase.Click Create Power Spectral Density Factors to define power spectral density factors.
Autocorrelation Function Time Lag	Specifies an Autocorrelation Function Time Lag modeling object for the step or subcase. This modeling object sets the number of time lag intervals, starting time lag, and maximum time lag between two signals for autocorrelation. Autocorrelation Function Time Lag provides the delay for autocorrelation between two signals (the original and its delayed copy).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.
Force Pre-Load
Pre-Load Type	Specifies whether to apply pressure and shear force result data from the Simcenter 3D Flow analysis to this step.Select Simcenter 3D Flow Pressure and Shear Forces from the list and then specify the location of the file. Click Browse to locate the thermal results file.This option corresponds to the Nastran FORCE bulk entry.	SOL 101 Linear Statics - Global Constraints (Subcase - Constraints)SOL 103 Response Dynamics (Subcase - Static Offset)SOL 106 Nonlinear Statics - Global Constraints (Subcase - Constraints)SOL 200 Design OptimizationSOL 200 Topology Optimization (Nastopt - Statics)SOL 601,106 Advanced Nonlinear StaticsSOL 601,129 Advanced Nonlinear TransientSOL 701 Explicit Advanced Nonlinear Analysis
Time Step Intervals	Defines the time step for the step or subcase. Time step definitions are stored as a solver-specific 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.This option corresponds to the Nastran TSTEP bulk entry.	SOL 109 Direct Transient ResponseSOL 112 Modal Transient Response
Forcing Frequencies	Defines the forcing frequencies for the step or subcase. Forcing frequency definitions are stored as solver-specific modeling objects.These options correspond to the Nastran FREQ, FREQ1, FREQ2, FREQ3, FREQ4, and FREQ5 bulk entries.Click to define forcing frequencies using the Modeling Objects Manager.	SOL 108 Direct Frequency ResponseSOL 108 Direct Frequency Response FunctionsSOL 108 Vibro-Acoustic Transfer VectorSOL 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 - Direct Frequency)
PEAKOUT Criteria	Defines the peakout criteria for the step or subcase.Direct/modal frequency peakout criteria definitions are stored as solver-specific modeling objects.Click to define the peakout criteria using the Modeling Objects Manager.This option corresponds to the Nastran PEAKOUT bulk entry.	SOL 108 Direct Frequency ResponseSOL 108 Vibro-Acoustic Transfer Vector Response (Subcase - Frequency Response)SOL 111 Modal Frequency Response
Mode Selection	Specifies the mode numbers of the structural or fluid modes to consider for the response computation.This option is useful after you solve 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.	SOL 200 Design Sensitivity Analysis (structural analysis, DSA - Modal Frequency and DSA - Modal Frequency Response Functions)
Damping TypeNote: For vibro-acoustic analyses, you can specify separate structural and fluid damping values. These options appear under separate 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.	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)
Structural DampingCritical DampingAmplification Factor Damping	Specifies the modal damping value.For more information, see Additional magnitude options.	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)
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.	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.This option corresponds to the Nastran DCONSTR bulk entry.	SOL 200 Design Optimization
Range of Forcing Frequencies (FREQV)
Enable Frequency Range	Controls the 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.This option corresponds to the Simcenter Nastran FREQV bulk entry.	SOL 108 Vibro-Acoustic Transfer Vector Response
Minimum Frequency	Appears when Enable Frequency Range is checked.Sets the lower bound of the frequency range.
Maximum Frequency	Appears when Enable Frequency Range is checked.Sets the upper bound of the frequency range.
Enforced Motion
Enforced Motion Method	Specifies the enforced motion.SPCDLets you directly specify displacements, velocities, or accelerations through SPC/SPC1/SPCD data.For more information, see The SPC/SPCD Methods.Large MassSpecifies the large mass and large mass moment of inertia values. Artificial masses attached to the structure at the degrees-of-freedom where the motion is to be enforced. These large masses should be in order of magnitude, such that larger than the total mass or the moment of inertia of the structure.For more information, see The Large Mass Method	SOL 108 Direct Frequency Response FunctionsSOL 111 Modal Frequency Response Functions
Mass	Specifies the artificial masses to be attached to the structure at the degrees-of-freedom where the motion is to be enforced.
Mass Moment of Inertia	Specifies the mass moment of inertia for the assigned larger mass of the structure.
Time Step Definition
End Time	Specifies the end time for the step. The sequence of steps is based on the End Time that you define for each step.You control the time steps in a solution step by specifying the End Time and Number of Increments for the step. The time steps for a solution step are determined by:time steps = (current solution step End Time – the previous solution step End Time) / Number of IncrementsThis option corresponds to the Tend parameter of the TSTEP1 bulk entry.	SOL 401 Multi-Step Nonlinear (Nonlinear Statics)SOL 402 Multi-Step Nonlinear Kinematics (Nonlinear Statics, Nonlinear Dynamics)
Number of Increments	Sets the number of increments in a solution step. If you set an end time, this option corresponds to the Ninc parameter of the TSTEP1 bulk entry.	SOL 401 Multi-Step Nonlinear (Nonlinear Statics, Preload)SOL 402 Multi-Step Nonlinear Kinematics (Nonlinear Statics, Nonlinear Dynamics, Preload)
Output Flag	Specifies the time points at which the software writes the results to the results file.Requested IncrementsOutputs data at each time step increment. Solution Step End TimeOutputs data only at the End Time for the current solution step.All TimesOutputs data at all time steps.Skip FactorOutputs data at the time step interval you specify.	SOL 401 Multi-Step Nonlinear (Nonlinear Statics, Preload)SOL 402 Multi-Step Nonlinear Kinematics (Nonlinear Statics, Nonlinear Dynamics, Preload (end time or all times).
Skip Factor	Appears when Output Flag is set to Skip Factor.Sets the step interval at which the software writes the results to the results file. For example, if you specify 5, the software outputs the results at every fifth time step.	SOL 401 Multi-Step Nonlinear (Nonlinear Statics, Preload)SOL 402 Multi-Step Nonlinear Kinematics (Nonlinear Statics, Nonlinear Dynamics)
Enable Bolt Sequencing	Controls whether all bolt pre-loads are applied at once, or if they are sequenced.When this is selected, the order in which the bolt pre-loads appear in the Loads container of the preload step defines the BOLTSEQ bulk entry.	SOL 401 Multi-Step Nonlinear (Preload)
Boundary Condition Control Variables
Evaluation Time	Specifies the value used to evaluate a time-dependent, or frequency-dependent boundary condition when you use the boundary condition in a solution that does not support dependent boundary conditions.The software first uses the field evaluation value for the step or subcase to determine the loading value. If no field evaluation value is defined for the step or subcase, the software uses the field evaluation value for the solution.	SOL 101 Linear Statics - Global Constraints (Subcase - Constraints)SOL 101 SuperelementSOL 103 Response DynamicsSOL 105 Linear BucklingSOL 106 Nonlinear Statics - Global Constraints (Subcase - Constraints)SOL 108 Direct Frequency ResponseSOL 108 Direct Frequency Response FunctionsSOL 108 Vibro-Acoustic Transfer Vector Response (Subcase - Frequency Response)SOL 111 Modal Frequency ResponseSOL 111 Modal Frequency Response FunctionsSOL 112 Modal Transient ResponseSOL 144 Static Aeroelastic ResponseSOL 153 Steady State Nonlinear Heat TransferSOL 200 Design OptimizationSOL 200 Design Sensitivity Analysis (vibro-acoustic analysis, DSA - Modal Frequency and DSA - Modal Frequency Response Functions)SOL 200 Topology Optimization
Evaluation Frequency		SOL 101 Linear Statics—Global Constraints, Subcase ConstraintsSOL 101 SuperelementSOL 103 Response DynamicsSOL 105 Linear BucklingSOL 106 Nonlinear Statics—Global Constraints, Subcase ConstraintsSOL 109 Direct Transient ResponseSOL 111 Modal Frequency Response Functions (Subcase-Statics)SOL 112 Modal Transient ResponseSOL 129 Nonlinear Transient ResponseSOL 144 Static Aeroelastic ResponseSOL 153 Steady State Nonlinear Heat TransferSOL 200 Design OptimizationSOL 200 Topology OptimizationSOL 401 Multi-Step Nonlinear (Nonlinear Statics, Preload)SOL 402 Multi-Step Nonlinear Kinematics (Nonlinear Statics, Nonlinear Dynamics, Preload)SOL 601,106 Advanced Nonlinear StaticsSOL 601,129 Advanced Nonlinear TransientSOL 701 Explicit Advanced Nonlinear Analysis
File Reference Subcase Id	Sets the subcase ID that corresponds to a subcase in an external result file, such as an HDF5 file.When you do not specify a value, the software uses the default subcase ID 1.	SOL 108 Vibro-Acoustic Transfer Vector Response (Subcase - Frequency Response)SOL 200 Design Sensitivity Analysis (Simcenter Nastran vibro-acoustic analysis, DSA - Modal Frequency)
Harmonics to Compute
Harmonics to Compute	Specifies the harmonic indexes to compute.To compute all harmonic indexes, select All Harmonics.To create a set of harmonic indexes to compute, select Specify Harmonics, and then create a modeling object to identify each index.Note: A separate modal solution is computed for each index. This defines a set number that contains only one unique harmonic to solve. If you want to solve several harmonics, you must define a separate cyclic modes subcase per harmonic to solve.This option corresponds to the Nastran HARMONICS case control command.	SOL 401 Multi-Step Nonlinear (Cyclic Modes)SOL 402 Multi-Step Nonlinear Kinematics (Cyclic Modes)
Harmonics Set	Appears when Harmonics to Compute is set to Specify Harmonics.Lets you create a set of one or more harmonic indexes. 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.This option corresponds to the Nastran HARMONICS case control command.	SOL 401 Multi-Step Nonlinear (Cyclic Modes)SOL 402 Multi-Step Nonlinear Kinematics (Cyclic Modes)
Harmonics Output
Harmonics Output	Specifies the harmonic indexes that you want to view in the output.To output all harmonic indexes, select All Harmonics. To output a set of harmonic indexes to compute, select Specify Harmonics, and then create a modeling object to identify each index. This option corresponds to the Nastran HOUTPUT case control command.	SOL 401 Multi-Step Nonlinear (Cyclic Modes)SOL 402 Multi-Step Nonlinear Kinematics (Cyclic Modes)
Harmonics Set	Appears when Harmonics to Output is set to Specify Harmonics.Lets you create a set of one or more harmonic indexes. 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.This option corresponds to the Nastran HOUTPUT case control command.	SOL 401 Multi-Step Nonlinear (Cyclic Modes)SOL 402 Multi-Step Nonlinear Kinematics (Cyclic Modes)
Aerodynamic Symmetry
Aerodynamic Symmetry XY	Specifies 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	Specifies 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

How do I

Create or modify a solution

Create or modify a solution step or subcase

Learn more

Solutions

Look up more details

Power Spectral Density Factors dialog box (Nastran)

Autocorrelation Function Time Lag dialog box (Nastran)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Solution Step/Subcase dialog box (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 } });