Solution dialog box (Nastran), Parameters page

Option	Corresponding Nastran syntax	Supported Nastran solutions	Description
Parameters	PARAM bulk entry	SOL 402 Multi-Step Nonlinear Kinematics	Select an existing solution parameters modeling object from the list or click Create Modeling Object to create a new solution parameters modeling object.Click Edit to edit the selected solution parameters modeling object.For more information, see Specifying parameters for Nastran analyses.
Large Strains	PARAM,LGSTRN	SOL 402 Multi-Step Nonlinear KinematicsSOL 601,106 Advanced Nonlinear StaticsSOL 601,129 Advanced Nonlinear TransientSOL 701 Explicit Advanced Nonlinear Analysis	Controls the strain formulation for Simcenter Nastran advanced nonlinear analyses.If you clear the Large Strains check box, Simcenter Nastran assumes a small strain formulation.For SOL 402, clearing the Large Strains check box sets the default stress-strain measure to Biot Strain, Biot Stress (Engineering).If you select the Large Strains check box, Simcenter Nastran assumes large strains, displacements, and rotations. Large strain formulation is only applicable to 2D axisymmetric, plane strain, 3D solid and single layer shell elements (except 8-node shells).For SOL 402, selecting the Large Strains check box sets the default stress-strain measure to Log Strain, Cauchy Stress (True).
Large Displacements	PARAM,LGDISP	SOL 402 Multi-Step Nonlinear KinematicsSOL 414,103 Eigenvalues and Superelement ReductionSOL 601,106 Advanced Nonlinear StaticsSOL 601,129 Advanced Nonlinear Transient	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.
Material Nonlinearity	PARAM,MATNL	SOL 402 Multi-Step Nonlinear Kinematics	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. See PARAM,MATNL for more information.
Flat Shell Rz Stiffness Factor	PARAM,K6ROT	SOL 402 Multi-Step Nonlinear KinematicsSOL 414,101 ManeuversSOL 414,103 Eigenvalues and Superelement ReductionSOL 414,110 Complex Modal AnalysisSOL 414,111 Harmonic AnalysisSOL 414,129 Transient Analysis	Specifies the stiffness to add to the normal rotation for CQUAD4 and CTRIA3 elements. To suppress singularities, a value between 1.0 and 100.0 is recommended.See PARAM,K6ROT for more information.
Number of Layers	PARAM,NLAYERS	SOL 402 Multi-Step Nonlinear KinematicsSOL 414,129 Transient Analysis	Sets the number of layers used to integrate through the thickness of CQUAD4 and CTRIA3 elements with isotropic material properties. A larger value gives greater accuracy at the cost of computing time and storage requirements.See PARAM,NLAYERS for more information.
OP2 Format (OP2FMT)	PARAM,OP2FMT	SOL 402 Multi-Step Nonlinear Kinematics	Specifies the format of the OP2 file (64-bit or 32-bit).Note: The 32-bit format does not support restarts with intermediate results files.See PARAM,OP2FMT for more information.
Grid Point Normals Generation Tolerance (SNORM)	PARAM,SNORM	SOL 402 Multi-Step Nonlinear Kinematics	Controls the smoothing of shell elements by providing a threshold angle. Use this option to take into account the curvature effects of elements that are defined only by corner nodes.For shell elements with an angle below the value you enter, the software computes a mean normal for the adjacent shell elements. For shell elements with an angle above the value you enter, the software retains one normal per node per element.Smoothing is enabled by default and set to 20 degrees. To disable smoothing for shell elements, set Grid Point Normals Generation Tolerance to 0.See PARAM,SNORM for more information.
Rayleigh Damping
**Mass Scale Factor (Real)**Mass Scale Factor (Imaginary)	PARAM,ALPHA1	SOL 402 Multi-Step Nonlinear KinematicsSOL 414,103 Eigenvalues and Superelement ReductionSOL 414,110 Complex Modal AnalysisSOL 414,111 Harmonic AnalysisSOL 414,129 Transient AnalysisSOL 601,106 Advanced Nonlinear StaticsSOL 601,129 Advanced Nonlinear TransientSOL 701 Explicit Advanced Nonlinear Analysis	Controls the specification of Rayleigh damping. Lets you specify the complex scale factor that Nastran applies to the mass matrix.For more information, see the Advanced Nonlinear Solution—Theory and Modeling Guide.
**Stiffness Scale Factor (Real)**Stiffness Scale Factor (Imaginary)	PARAM,ALPHA2	SOL 402 Multi-Step Nonlinear KinematicsSOL 414,103 Eigenvalues and Superelement ReductionSOL 414,110 Complex Modal AnalysisSOL 414,111 Harmonic AnalysisSOL 414,129 Transient AnalysisSOL 601,106 Advanced Nonlinear StaticsSOL 601,129 Advanced Nonlinear Transient	Controls the specification of Rayleigh damping. Lets you specify the complex scale factor that Nastran applies to the stiffness matrix.For more information, see the Advanced Nonlinear Solution—Theory and Modeling Guide.
Modal Damping
PARAM,MDLDAMP	PARAM,MDLDAMP	SOL 110 Modal Complex Eigenvalue AnalysisSOL111 Modal Frequency Response AnalysisSOL 112 Modal Transient Response AnalysisSOL 145 Aeroelastic FlutterSOL 200 Design Optimization and Sensitivity	Controls the specification of equivalent modal structural damping.For more information see M – Parameters
PARAM,KDAMP	PARAM,KDAMP	SOL 110 Modal Complex Eigenvalue AnalysisSOL111 Modal Frequency Response AnalysisSOL 112 Modal Transient Response AnalysisSOL 145 Aeroelastic FlutterSOL 200 Design Optimization and Sensitivity	Controls the specification of modal damping.For more information see K – Parameters
Damping
Overall Structural Damping	PARAM,G	All SOL 414 Rotor Dynamics solutions except SOL 414,101 Maneuvers	Specifies structural damping
Overall Structural Damping Dominant Frequency	PARAM,W3	All SOL 414 Rotor Dynamics solutions except SOL 414,101 Maneuvers	Sets the frequency at which the overall structural damping is converted to viscous damping
Element Structural Damping Dominant Frequency	PARAM,W4	All SOL 414 Rotor Dynamics solutions except SOL 414,101 Maneuvers	Sets the frequency at which element structural damping is converted to viscous damping
Recombination
Fourier Harmonic Post-Processing Recombination Mode (FHPOST)	PARAM,FHPOST	SOL 402 Multi-Step Nonlinear KinematicsAll SOL 414 Rotor Dynamics solutions	Specifies the recombination option for 3D results output when the axisymmetric Fourier elements are requested with the Harmonics Set modeling object.
Number of Recombined Elements per 90 Degrees (FHPNST)	PARAM,FHPNST	SOL 402 Multi-Step Nonlinear KinematicsAll SOL 414 Rotor Dynamics solutions	Specifies the number of angle increments in a 90 degree quadrant in which the software computes the 3D harmonic results for the axisymmetric Fourier elements. This output displays the non-axisymmetric results on a full revolute model.
Postprocessing
.f06 Output (SEMATPRT)	PARAM,SEMATPRT	SOL 414,103 Eigenvalues and Superelement Reduction	Appears when Computation Options is set to Superelement Reduction.Specifies which matrices are written to the .f06 file.Reduced MatricesFor a fixed reference frame, prints stiffness, mass, gyroscopic, and hysteretic damping matrices.For a rotating reference frame, prints stiffness, mass, Coriolis, hysteretic damping, and centrifugal matrices.Reduced Matrices and Implicit LoadPrints the same matrices as Reduced Matrices but with the addition of element loading matrices.

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), Parameters 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 } });