Solution dialog box (Nastran), Bulk Data page

Option	Description	Corresponding Nastran syntax	Supported Nastran solutions
Integrated Load Monitor Points	Specifies the Monitor Point - Element Monitor and Monitor Point - Sums Grid Point Forces modeling objects. For more information, see Generating specific component output for elements and nodal sums of forces and moments (Simcenter Nastran).	MONPNT2 and MONPNT3	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)
Fluid-Structure Interface Parameters	Specifies the Fluid-Structure Interface Parameters modeling object to define parameters that model the fluid-structure interface (coupling) for vibro-acoustic analyses.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.If the list is extensive, click More Options to search for a particular modeling object or filter the list. For more information, see Filter options.	ACMODL	SOL 103 Real EigenvaluesSOL 107 Direct Complex EigenvaluesSOL 108 Direct Frequency ResponseSOL 108 Direct Frequency Response FunctionsSOL 108 Vibro-Acoustic Transfer Vector (Simcenter Nastran only)SOL 110 Modal Complex EigenvaluesSOL 111 Modal Frequency ResponseSOL 111 Modal Frequency Response FunctionsSOL 111 Vibro-Acoustic Transfer Vector (Simcenter Nastran only)SOL 200 Design Sensitivity Analysis (vibro-acoustic analysis)
Design Variables	Sets the physical attributes in the FEM that the software can modify in its search for an improved design. It can vary physical properties, material properties, and element properties. The design variable modeling object also defines the relationship between a variable and the corresponding property of the model.	DESVAR and DVPREL1, DVMREL1, or DVCREL1	SOL 200 Design Optimization
Design Optimization Parameters	Specifies the parameters that control the optimization analysis.For more information, see Control the design optimization output.	DOPTPRM	SOL 200 Design OptimizationSOL 200 Design Sensitivity Analysis
Topology Optimization Parameters (DOPTPRM)	Specifies the design optimization parameters modeling object 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.	DOPTPRM	SOL 200 Topology Optimization
Maximum Number of Design Cycles (DESMAX)	Sets the number of number of topology optimization design cycles to perform.Note: If you select a modeling object from the Topology Optimization Parameters (DOPTPRM) list that has a value defined for DESMAX, that value overrides the value specified for Maximum Number of Design Cycles (DESMAX).	DOPTPRM	SOL 200 Topology Optimization
Penalty Law (DMRLAW)	Specifies the relation between the material properties and the normalized material density.LinearThe elements' stiffness values scale linearly with their density. This often produces topology optimization results with many intermediate material density values, which might not be desirable.SIMPThe stiffness of the elements is calculated using the following equation, where p is the value specified for SIMP Penalty Value.RAMPThe stiffness of the elements is calculated using the following equation, where q is the value specified for RAMP Penalty Value.This option can improve convergence for eigenfrequency-related optimization problems.LATTICELets you specify a lattice structure for 3D printing.	DMRLAW	SOL 200 Topology Optimization
SIMP Penalty Value	Appears when Penalty Law (DMRLAW) is set to SIMP.Sets the value for p in the SIMP equation.	DMRLAW	SOL 200 Topology Optimization
RAMP Penalty Value	Appears when Penalty Law (DMRLAW) is set to RAMP.Sets the value for q in the RAMP equation.	DMRLAW	SOL 200 Topology Optimization
Lattice Structure Type	Appears when Penalty Law (DMRLAW) is set to LATTICE.Specifies the lattice structure to use.For more information, see Lattice structures.	DMRLAW	SOL 200 Topology Optimization
Recovery Option (NASPRT)	Specifies which design cycles to include in the results.Initial and BestInclude results for Design Cycle 0 (no optimization) and the last design cycle, which should be the best optimization results.Initial with Skipped CyclesInclude results for Design Cycle 0 and all the design cycles that were not skipped (as determined by the value for Cycle Skip Count).Initial and All ImprovedInclude Design Cycle 0 and every cycle that shows an improvement over the previous cycle.Limiting the number of design cycles reduces the size of the .op2 file.Note: If you select a modeling object from the Parameters list that has a value defined for NASPRT, that value overrides your selection in the Recovery Option (NASPRT) list.	NASPRT	SOL 200 Topology Optimization
Cycle Skip Count	Appears when Recovery Option (NASPRT) is set to Initial with Skipped Cycles.Sets which design cycles to skip.The count begins with Design Cycle 0, and that design cycle is always included in the results.If you set Cycle Skip Count to 1, no cycles are skipped, so you get results for Design Cycles 0, 1, 2, 3, and so on. If you set Cycle Skip Count to 5, the cycles up to every fifth one are skipped, so you get results for Design Cycles 0, 4, 9, 14, and so on.Setting Cycle Skip Count to 0 includes only the results for Design Cycle 0 (no optimization) and the last design cycle.	NASPRT	SOL 200 Topology Optimization
Augmented Time Step****Augmented Time Step List	Specifies additional time step intervals. If you omit the Augmented Time Step modeling object, you have only a single interval that ends at the subcase end time.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.	TSTEP1	SOL 401 Multi-Step NonlinearSOL 402 Multi-Step Nonlinear KinematicsSOL 414,129 Transient Analysis
Parameters	Specifies the PARAM bulk entry for the solution.For more information, see Specifying parameters for Nastran analyses.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.If the list is extensive, click More Options to search for a particular modeling object or filter the list.Note: If you select a solution parameters modeling object that has a value defined for NASPRT, that value overrides your selection in the Recovery Option (NASPRT) list.	PARAM bulk entry	All solutions except the following:SOL 414,101 ManeuversSOL 414,103 Eigenvalues and Superelement ReductionSOL 414,110 Complex Modal AnalysisSOL 414,111 Harmonic ResponseSOL 414,129 Transient Response
Dynamic Data Recovery (DDRMM)	Specifies the method to use for recovering results data.If you clear this check box, this information is not written to the input file.Mode Displacement MethodRecovers dynamic physical responses from modal responses. This method assumes that the physical responses are the linear combination of modal contributions from normal modes.Matrix MethodRecovers stress, displacements, forces, and strains directly from the modal solution frequency response. Select this option when the number of subcases is much larger than the number of modes and when the solution contains very few output requests.	PARAM, DDRMM	SOL 111 Modal Frequency Response (structural and vibro-acoustic analyses)SOL 111 Modal Frequency Response Functions (structural and vibro-acoustic analyses)SOL 111 Vibro-Acoustic Transfer Vector (Simcenter Nastran only)SOL 200 Design Sensitivity Analysis
Inertia Relief (INREL)	Controls the calculation of inertia relief or enforced acceleration.For more information, see:Data Recovery Operations in SubDMAP SEDISPBuckling Analysis in SubDMAP MODERSAutomatic Inertia ReliefNote: If you select a solution parameter that has a value defined for INREL, that value overrides the state of this check box.	PARAM, INREL	SOL 101 Linear Statics - Global ConstraintsSOL 101 Linear Statics - Subcase ConstraintsSOL 200 Design OptimizationSOL 200 Topology OptimizationNote: For SOL 200 Design Optimization and SOL 200 Topology Optimization solutions, only statics subcases support automatic inertia relief.In addition, if your topology optimization design objective is for compliance, do not select this check box. If you do, the solve will fail.
Flat Shell Rz Stiffness Factor (K6ROT)	Lets you specify the stiffness to add to the normal rotation for CQUAD4 and CTRIA3 elements. This is an alternate method to suppress the grid point singularities. It is primarily intended for geometric nonlinear analysis. A value between 1.0 and 100.0 is recommended to suppress singularities. A large value may be required in nonlinear and eigenvalue analyses. This parameter is ignored for CQUADR, CTRIAR, CQUAD8, and CTRIA6 elements. K6ROT is forced to 0 when only membrane elements exist.	PARAM, K6ROT	SOL 101 — Single constraintSOL 101 — Multi constraintSOL 103 Real EigenvaluesSOL 103 Response DynamicsSOL 105 Linear BucklingSOL 106 Nonlinear StaticsSOL 108 Direct Frequency ResponseSOL 108 Direct Frequency Response FunctionsSOL 108 Vibro-Acoustic Transfer Vector (Simcenter Nastran only)SOL 109 Direct Transient ResponseSOL 111 Modal Frequency ResponseSOL 111 Modal Frequency Response FunctionsSOL 111 Vibro-Acoustic Transfer Vector (Simcenter Nastran only)SOL 112 Modal Transient ResponseSOL 144 Static Aeroelastic ResponseSOL 145 Aeroelastic FlutterSOL 200 Design Sensitivity AnalysisSOL 200 Topology Optimization
Rotor Dynamics CSV Output	Directs Simcenter Nastran to write a .csv file that contains the complex eigenvalue analysis results. The .csv file is typically used to create a Campbell diagram.	PARAM,ROTCSV	SOL 107 Direct Complex EigenvaluesSOL 110 Modal Complex Eigenvalues
Rigid Body Modes Below	In a Response Dynamics analysis, this option identifies rigid body modes for computing the viscous damping ratio matrix. That matrix is written to the OP2 file when RSOPT=1. Nastran considers frequencies below the LAMLIN value a rigid body mode. The column and rows of the viscous damping ratio matrix associated with the rigid body will be set to zero.	PARAM,LAMLIM	SOL 103 Response Dynamics
Large Displacements	In a nonlinear analysis, for all nonlinear element types which have a large displacement capability, controls whether Nastran assumes they have large displacement effects (updated element coordinates and follower forces).See PARAM,LGDISP for more information.	PARAM,LGDISP	SOL 106 Nonlinear StaticsSOL 129 Nonlinear Transient ResponseSOL 153 Steady State Nonlinear Heat TransferSOL 401 Multi-Step Nonlinear
Material Nonlinearity	Enables material nonlinear capabilities (plasticity, creep, and damage material properties for cohesive elements) for all subcases. Selecting this check box also includes material properties for progressive ply failure.When this check box is selected, you can disable plasticity and creep for individual subcases using a Nonlinear Control Parameters - Subcase modeling object. You cannot disable damage material properties or progressive ply failure for individual subcases.When this check box is cleared, plasticity and creep are not included in the solve regardless of creep and plasticity settings in the Nonlinear Control Parameters - Subcase modeling object.	PARAM,MATNL	SOL 401 Multi-Step Nonlinear
Modal Damping Conversion for Structure (KDAMP)	Specifies the modal damping approach to use.If you clear this check box, this information is not written to the input file.This option is useful for models for which you have no knowledge of physical damping. For response calculations, both viscous and structural damping are used. With a modal approach, so you can specify modal viscous and modal structural damping ratios for each active normal mode.See Modal damping for more information.	KDAMP	SOL 111 Modal Frequency Response (vibro-acoustic analysis)SOL 111 Modal Frequency Response Functions (vibro-acoustic analysis)SOL 111 Vibro-Acoustic Transfer Vector (Simcenter Nastran only)SOL 200 Design Sensitivity Analysis
Shell Property Structural Damping Coefficient (SHLDAMP)	Specifies how the structural damping coefficient (GE) defined on the PSHELL material is used.If you clear this check box, this information is not written to the input file.**Obtained From Material (SAME)**The structural damping coefficient (GE) defined on a PSHELL MID1 material is used by all MIDi for that PSHELL.**Obtained From Each Material (DIFF)**The structural damping coefficient (GE) defined on each PSHELL MIDi is used. Any structural damping coefficient (GE) values that are blank default to zero.	SHLDAMP	SOL 200 Design Sensitivity Analysis
Mass Matrix Coupling (COUPMASS)	Specifies how to handle both structural and nonstructural mass for the following elements: CBAR, CBEAM, CONROD, CHEXA, CPENTA, CPYRAM, CQUAD4, CQUAD8, CQUADR, CQUADX4, CQUADX8, CRAC2D, CRAC3D, CROD, CTETRA, CTRAX3, CTRAX6, CTRIA3, CTRIA6, CTRIAR, and CTUBE.If you clear this check box, this information is not written to the input file.LumpedGenerates lumped mass matrices (translational components only) for the elements.CoupledGenerates coupled mass matrices for elements with coupled mass capability.Note: CBEND elements are always generated with coupled mass and are not affected by this setting.	COUPMASS	SOL 200 Design Sensitivity Analysis
Residual Vector Correction for Massless DOFs (RVMASS)	Specifies whether to add a small mass to DOFs with stiffness.If you clear this check box, this information is not written to the input file.Selecting Yes from this list does not affect the mass of the model.	RVMASS	SOL 200 Design Sensitivity Analysis
**Structural Damping (G)**Overall Structural Damping (G)	Sets the uniform structural damping coefficient used in the formulation of dynamics problems.	PARAM,G	SOL 108 Direct Frequency Response (structural and vibro-acoustic analyses)SOL 108 Direct Frequency Response Functions (structural and vibro-acoustic analyses)SOL 108 Vibro-Acoustic Transfer Vector (Simcenter Nastran only)SOL 109 Direct Transient ResponseSOL 111 Modal Frequency Response (vibro-acoustic analysis)SOL 111 Modal Frequency Response Functions (vibro-acoustic analysis)SOL 111 Vibro-Acoustic Transfer Vector (Simcenter Nastran only)SOL 200 Design Sensitivity Analysis
Overall Structural Damping Dominant Frequency (W3)	Specifies the viscous damping matrix for transient analysis or for interfacing with external programs via the ADAMSMNF and MBDEXPORT case control commands. For more information, see PARAM,W3.	PARAM,W3	SOL 109 Direct Transient Response
Element Structural Damping Dominant Frequency (W4)	Specifies the viscous damping matrix for transient analysis or for interfacing with external programs via the ADAMSMNF and MBDEXPORT case control commands. For more information, see PARAM,W4.	PARAM,W4	SOL 109 Direct Transient Response
Modal Damping for Fluid (KDAMPFL)	Controls whether the software computes Structural or Viscous damping for the fluid portion of the model.	KDAMPFL	SOL 111 Modal Frequency Response (vibro-acoustic analysis)SOL 111 Modal Frequency Response Functions (vibro-acoustic analysis)SOL 111 Vibro-Acoustic Transfer Vector (Simcenter Nastran only)
Overall Fluid Damping (GFL)	Sets the uniform fluid damping coefficient used in the formulation of dynamics problems.	GFL	SOL 108 Direct Frequency Response (Simcenter Nastran vibro-acoustic analysis)SOL 108 Direct Frequency Response Functions (Simcenter Nastran vibro-acoustic analysis)SOL 108 Vibro-Acoustic Transfer Vector (Simcenter Nastran only)SOL 111 Modal Frequency Response (Simcenter Nastran vibro-acoustic analysis)SOL 111 Modal Frequency Response FunctionsSOL 111 Vibro-Acoustic Transfer Vector (Simcenter Nastran only)SOL 200 Design Sensitivity Analysis (vibro-acoustic analysis)Note: SOL 108 and SOL 111 solutions are also supported that contain models with Automatically Matched Layer (AML) boundary conditions.
Grid Point Normal Generation Tolerance (SNORM)	Sets a surface normal vector at a node for CQUAD4, CQUADR, CTRIA3, and CTRIAR shell elements.	SNORM	SOL 200 Design Sensitivity Analysis
Skip Solving the Structural DOFs	When surface vibrations on the structure are known and defined as an input excitation, you may only need the structural DOFs in order to enforce this loading to the acoustic mesh.You can set the SPCSTR parameter to YES to constrain the structural DOFs in the analysis set, but only after the structural excitation is transferred over to the fluid. It is set to NO as default value.	SPCSTR	SOL 108 Direct Frequency Response (Simcenter Nastran vibro-acoustic analysis)SOL 108 Direct Frequency Response Functions (Simcenter Nastran vibro-acoustic analysis)SOL 111 Modal Frequency ResponseSOL 111 Modal Frequency Response Functions
Enable Adaptive Order for Acoustic Elements	Enables the Finite Element Method Adaptive Order (FEMAO) method.For more information, see Finite Element Method Adaptive Order (FEMAO).Note: For vibro-acoustic analyses using FEMAO and distributed memory parallel (DMP) processing, there may not be enough memory assigned to Simcenter Nastran by default. This can result in an error, and an incorrect error message that does not indicate memory shortage. A workaround may be to increase the memory using the memorydefault keyword. You can set this additional keyword in the nastran Command Keywords group in the Solver Parameters dialog box.For information on memorydefault, see Managing Memory in the Simcenter Nastran Installation and Operations Guide.		SOL 108 Direct Frequency ResponseSOL 108 Direct Frequency Response Functions (Simcenter Nastran vibro-acoustic analysis)SOL 111 Modal Frequency ResponseSOL 111 Modal Frequency Response Functions
Adaptation Rule (ACADAPT)	Specifies the refinement type.CoarseFour elements per wavelength.StandardEight elements per wavelength.FineTwenty elements per wavelength.The adaptation rule determines the order of elements to be used at low and high frequencies.Adaption rule uses:Higher-order acoustic shape functions (higher number of DOFs per element) at high frequencies, large elements, or a combination of both.Lower-order acoustic shape functions (lower number of DOFs per element) at low frequencies, small elements, or a combination of both.The adaptation rule FINE results in more higher order elements to be used at lower frequencies compared to the adaption rule COARSE for the same mesh.The order adaptation also takes into account the local (per element) speed of sound. In two geometrically identical elements, the one with lower speed of sound will go to higher orders at lower frequencies compared to the other element.Provides more accurate results and faster solving time by adapting the computational effort to the complexity of the analysis.	ACADAPT	SOL 108 Direct Frequency ResponseSOL 108 Vibro-Acoustic Transfer Vector (Simcenter Nastran only)SOL 111 Modal Frequency ResponseSOL 111 Vibro-Acoustic Transfer Vector (Simcenter Nastran only)
Order Limit (ACORDER)	Specifies the highest polynomial order limit.The order limit determines the range of element orders that the FEMAO will use in its adaptive solving.DefaultLets you specify the default lowest (2) and/or highest (10) element order you want the FEMAO method to use.MinimumLets you enter the lowest element order you want the FEMAO method to use.MaximumLets you enter the highest element order you want the FEMAO method to use.Minimum and MaximumLets you enter both the lowest and highest element order you want the FEMAO method to use.	ACORDER
Minimum Order	Appears when Order Limit is set to Minimum or to Minimum and Maximum.Sets the lowest polynomial order you want the FEMAO method to use.
Maximum Order	Appears when Order Limit is set to Maximum or to Minimum and Maximum.Sets the highest polynomial order you want the FEMAO method to use.
FEMAO Quality Results (GPACAO)	Available when FEMAO is enabled. Enable Adaptive Order for Acoustic ElementsEnables you to solve the solution with the model check deactivated.	GPACAO
FEMAO Stabilization (STABAO)	Available when FEMAO is disabled. Enable Adaptive Order for Acoustic ElementsYou activate FEMAO Stabilization (STABAO) to correct dispersion at high frequencies by stabilizing computation at the element Gauss points.	STABAO
FEM Stabilization (STABFEM)	Available when Enable Adaptive Order for Acoustic Elements is cleared. Note: Simcenter Nastran Acoustic SOL 108 Acoustic Transfer Vector and SOL 111 Modal Frequency Response do not support FEMAO, so the Enable Adaptive Order for Acoustic Elements option is not available. You can apply stabilization to a FEM solution directly.Corrects dispersion at high frequencies by stabilizing computation at the element Gauss points.	STABFEM	SOL 108 Acoustic Transfer Vector (Simcenter Nastran acoustic analysis)SOL 108 Direct Frequency Response (Simcenter Nastran acoustic and vibro-acoustic analyses)SOL 108 Direct Frequency Response Functions (Simcenter Nastran vibro-acoustic analysis)SOL 111 Modal Frequency Response (Simcenter Nastran acoustic and vibro-acoustic analyses)SOL 111 Modal Frequency Response Functions (Simcenter Nastran vibro-acoustic analysis)
DOF Sets	Specifies the DOF set to use.Select an existing DOF set from the list or click New DOF Set to create a new one.If the list is extensive, click More Options to search for a particular DOF set or filter the list.	ASET, BNDFIX, BNDFREE, BSET, CSET, OMIT, QSET, RVDOF SUPORT, USET	All solutions except the following:SOL 402 Multi-Step Nonlinear KinematicsSOL 414 Eigenvalues and Superelement Reduction
CFAST/CWELD Connection Parameters	Lets you select or create a CFAST/CWELD Connection Parameters modeling object.For more information, see Defining properties and parameters for CFAST/CWELD connections.	SWLDPRM bulk entry	All solutions except the following:SOL 402 Multi-Step Nonlinear Kinematics
Frequency Response Solution Options	Appears when the analysis type is set to Structural, or when the analysis type is set to Vibro-Acoustic and the Enable Adaptive Order for Acoustic Elements check box is cleared.Lets you select or create a Frequency Response Solution Options modeling object.	SLVCNTL bulk entry	SOL 108 Direct Frequency Response SOL 108 Direct Frequency Response Functions SOL 111 Modal Frequency ResponseSOL 111 Modal Frequency Response Functions
User Defined Text	Lets you insert comments or include a file in the bulk data section of your Nastran input file. For more information, see Customizing a Nastran input file with user defined text.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.If the list is extensive, click More Options to search for a particular modeling object or filter the list.Note: For SOL 200 Topology Optimization solutions, the user-defined text modeling object cannot include a value for DMRLAW. Simcenter Nastran supports the use of only one DMRLAW value, and this is defined by Penalty Law (DMRLAW) in the Optimization Parameters subgroup.	$ or INCLUDE	All solutions
Solution Options	Lets you define solution parameters for the rotor dynamic 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.	ROTORD	SOL 414,101 ManeuversSOL 414,110 Complex Modal AnalysisSOL 414,111 Harmonic ResponseSOL 414,129 Transient Response
Reference System	Appears when Computation Options is set to Superelement Reduction.Specifies the reference frame for the rotor superelement. You must use the same type of reference frame in the analysis that uses the generated superelement.	ROTORD	SOL 414,103 Eigenvalues and Superelement Reduction
Aerodynamic Static Parameters	Lets you define aerodynamic static parameters for the static aeroelastic response 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.	AEROS	SOL 144 Static Aeroelastic Response
Trim Variables	Lets you define trim variables for the static aeroelastic response 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.	AESTAT	SOL 144 Static Aeroelastic Response

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), Bulk Data 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 } });