(1)

(2)

(3)

(4)

(5)

(6)

(7)

(8)

(9)

(10)

PARAM

N

V

Field

Contents

N

Name of Parameter.

V

Value of Parameter.

ACMODL12

Restores the ACMODL formulation used in version 12.0 and earlier for the Fluid-Structure Interface.

<YES, NO>
Default = NO

AGGPCH

To support output of the fluid-structure coupling matrix to the Punch (.pch) file as a matrix defined using DMIG data entry.

<YES, NO>
Default = NO

AKUSMOD

Use external fluid-structure coupling matrix generated by AKUSMOD.

<YES, NO>
Default = NO

ALPHA1

Adds Rayleigh damping to viscous damping for structural mesh.

<Real>
Default = 0.0

ALPHA2

Adds Rayleigh damping to viscous damping for structural mesh.

<Real>
Default = 0.0

ALPHA1FL

Adds Rayleigh damping to viscous damping for fluid mesh.

<Real>
Default = 0.0

ALPHA2FL

Adds Rayleigh damping to viscous damping for fluid mesh.

<Real>
Default = 0.0

AMLS

Use external AMLS eigenvalue solver.

<YES, NO>
Default = NO

AMLSMAXR

Used to determine singularities in the stiffness matrix for AMLS eigenvalue solver.

<Real>
Default = 1.0e-8

AMLSMEM

Defines the amount of memory in Gigabytes to be used by the external AMLS eigenvalue solver.

<Real>
No default

AMLSNCPU

Used to define the number of cpu’s to be used by the external AMLS eigenvalue solver.

Integer > 1
Default = 1

AMLSUCON

Constrain unconnected grids for AMLS eigenvalue solver.

<1, 0>
Default = 0

AMSE4CMS

Controls the alternate method for the creation of CMS superelements using the AMSES eigensolver.

<YES, NO>

AMSESLM

Indicates if the AMSES numerical mode for enforced motion based modal dynamic analysis with large mass method will be activated or not.

<YES, NO>
Default = NO

ASCOUP

Generates the fluid-structure coupling (area) matrix for use in the solution.

<YES, NO>
Default = YES

AUTOMSET

Automatically convert dependent degrees-of-freedom of rigid elements to independent degrees-of-freedom.

<YES, NO>
Default = NO

AUTOSPC

Automatically constrain degrees-of-freedom with no stiffness.

<YES, NO>
Default = YES

AUTOSPRT

Activate inertia relief and auto-support degree-of-freedom generation.

<1, 0>
Default = 1

BUSHRLMT

Issues a WARNING when the stiffness value for rotational components on the PBUSH entry exceeds the specified limit (BUSHRLMT).

<Real Number > 0.0>
Default = 1.0E+09

BUSHSTIF

Specifies a value to replace large stiffness values (>1.0E+07) input in field K of the PBUSH data entry.

<Real Number > 0.0>
No default

BUSHTLMT

Issues a WARNING when the stiffness value for translational components on the PBUSH entry exceeds the specified limit (BUSHTLMT).

<Real Number > 0.0>
Default = 1E+07

CB2

Scale factor for direct input damping matrices.

<Real>
Default = 1.0

CDITER

Controls the activation of MPC-based Fast Contact Analysis.

<Integer > 0>
Default = 0

CDPCH

Controls the printing of the final state of DMIG,CDSHUT for the constrained degrees of freedom at the gap interface to the PUNCH file for MPC-based Fast Contact Analysis.

<YES, NO>
Default = NO

CDPRT

Controls the printing of violations during intermediate iterations in MPC-based Fast Contact Analysis to the .out file.

<YES, NO>
Default = NO

CHECKEL

Activates element quality checking.

<NO, YES, FULL>
Default = YES

CHECKMAT

Activates material property checking.

<YES, NO, FULL>
Default = YES

CHKELSET

Specifies or excludes an element set from element quality check.

<Integer>
No default

CHKGPDIR

Activates gap direction alignment checking.

<YES, NO, WARN,
FULL, REVERSE>
Default = YES

CK2

Scale factor for direct input stiffness matrices.

<Real>
Default = 1.0

CK3

Specifies factors for the stiffness matrix produced by GENEL cards.

<Real>
Default = 1.0

CM2

Scale factor for direct input mass matrices.

<Real>
Default = 1.0

CMFTINIT

Defines lower threshold for *.HM.comp.cmf and *.HM.ent.cmf HyperMesh command files.

0.0 < Real < 1.0
Default = 0.0

CMFTSTEP

Defines step or interval value for *.HM.comp.cmf and *.HM.ent.cmf HyperMesh command.

0.0 < Real < 1.0
Default = 0.1

CMSALOAD

Controls the inclusion of mass contribution from the mass matrix stored in the PUNCH DMIG or the H3D DMIG files for the generation of RFORCE and Gravity Loads.

<YES, NO>
Default = YES

CMSDIRM

Allows flexible body generation when directional masses are defined in the input file.

<YES, NO>
Default = NO

CMSOFST

Consider shell offsets for flexbody generation.

<YES, NO>
Default = NO

COEFFC

Friction coefficient on curvatures for one-step stamping simulation.

<Real > 0.0>

COMP2SHL

Results of homogenization of composite properties.

<YES, NO, BULK>
Default = NO

CONTFEL

Activates Contact-friendly elements. This is recommended when second order solids/gaskets are used with contact analysis in OptiStruct.

<YES, NO, AUTO>
Default = AUTO

COUPMASS

Use coupled mass matrix approach for eigenvalue analysis.

<-1, 0, 1, YES, NO>
Default = NO

CP2

Scale factor for direct input load matrices.

<Real>
Default = 1.0

CSTEVAL

Use wall time based cost evaluation for Lanczos steps.

<YES, NO>
Default = YES

CSTOL

Specifies how many decimal digits may be lost to cancellation in one operation during the eigensolution process.

<Real>
Default = 3.5

CURVSHL2

Activates a correction to strain and stress calculation for second order shell elements (CQUAD8, CTRIA6) that takes into account strong curvature of the shell (relative to shell thickness).

<NO, YES>
Default = NO

DFREQ

Used to determine duplicate frequencies.

<Real>
Default = 10-5

DISIFMCK

Skip indefinite mass matrix check.

<YES, NO>
Default = NO

DISJOINT

Used to allow AMLS to handle disconnected parts. This can also be accomplished with PARAM, AMLSUCON.

<Integer>
Default = NONE

DSZERO

Sets a threshold (minimum absolute value) for the printing of Design Sensitivities.

Real ≥ 0.0
Default = 0.0

DUPTOL

Level of accuracy used in determining duplicate grids.

<0, 1, 2, 3, 4, 5>
Default = 0

EFFMAS

Outputs modal participation factors and effective mass for normal modes analyses.

<YES, NO, Integer>
Default = NO

EHD

Prints the inverse of the stiffness matrix created by static reduction to FORTRAN unit 3

<YES, NO>
Default = NO

ELASRLMT

Issues a WARNING when the stiffness value for rotational components on the CELAS2/4 or PELAS entry exceeds the specified limit (ELASRLMT).

<Real Number > 0.0>
Default = 1.0E + 09

ELASSTIF

Specifies a value to replace large stiffness values (>1.0E+07) input in field K of the PELAS data entry.

<Real Number > 0.0>
No default

ELASTLMT

Issues a WARNING when the stiffness value for translational components on the CELAS2/4 or PELAS entry exceeds the specified limit (ELASTLMT).

<Real Number > 0.0>
Default = 1E+07

ENFMOTN

Switch between relative and absolute displacement output in Modal Frequency Response Analysis with enforced motion.

<REL, ABS, TOTAL>
Default = ABS

ERPC

The speed of sound used in the ERP calculation.

Real > 0.0
Default = 1.0

ERPREFDB

The reference value in decibels (dB) used in ERP calculations.

Real > 0.0
Default = 1.0

ERPRHO

The fluid density used in ERP calculations.

Real > 0.0
Default = 1.0

ERPRLF

The Radiation Loss Factor used in ERP calculation.

Real > 0.0
Default = 1.0

EXCEXB

Controls the output of the AVL/EXCITE .exb file directly from OptiStruct.

<GMOT, SMOT, GMOTR, NO>

EXCOP2

This parameter controls the output of the AVL EXCITE _AVL.op2 file directly from OptiStruct.

<YES, NO>
Default = YES

EXCOUT

Output of condensed superelement information for AVL/EXCITE to the corresponding output files.

<-1, 0, 1, 3, 4, 5, 6>
Default = 0

EXPERTNL

Activates nonlinear expert system to aid in the convergence of small displacement nonlinear problems.

<YES, NO, CNTSTB, AUTO>
Default = AUTO

EXTOUT

EXTOUT controls the output of reduced matrices to external data files for use in subsequent analyses.

<DMIGPCH,
DMIGBIN, DMIGOP2, DMIGOP4>
Default = DMIGPCH

FASTCONT

Controls the activation of CONTACT/CGAP(G)-based Fast Contact. If this parameter does not exist in the input deck (default), Linear Gap Analysis is not activated.

<YES, NO>
Default = NO

FASTFR

Controls the activation of a faster, alternative method (FASTFR) for Modal Frequency Response Analysis.

<AUTO, YES, NO>

FFRS

Used to invoke the external FastFRS (Fast Frequency Response Solver).

<YES, NO>
Default = NO

FFRSLFREQ

Defines a frequency cut-off value in Hertz used to partition the structural system into low frequency and high frequency parts.

<Real>
Default = 1.0

FFRSMEM

Defines the amount of memory in Gigabytes to be used by the external FastFRS modal equation solver.

<Real>

FFRSNCPU

Defines the number of cpu’s to be used by the external FastFRS solver.

<INTEGER>
Default = number of cpu's used by OptiStruct.

FLEXH3D

Generates flexh3d files for flexible bodies in an MBD analysis.

<AUTO, YES, NO>
Default = AUTO

FLIPOK

Allows tetrahedral elements to invert during shape optimization.

<NO, YES>
Default = NO

FLLWER

Calculation of follower forces introduced by pressure loads and concentrated forces in large displacement nonlinear analysis.

<-1, 0, 1, 2, 3>
Default = 1

FRIC

Defines multiplier for K2PP reference.

<Real>
Default = 1.0

FZERO

Identifies the maximum frequency of a rigid body mode.

<Real>
Default = 0.1

G

Specifies the uniform structural damping coefficient for dynamic analyses.

<Real>
Default = 0.0

GE_MOD

Modifies specified GE values.

<Real or NO_GE>
No default

GFL

Specifies the uniform fluid damping coefficient for dynamic analyses.

<Real>
Default = 0.0

GMAR

Controls the accuracy of the external AMLS eigenvalue solution.

<Real>
Default = 1.1

GMAR1

Controls the accuracy of the external AMLS eigenvalue solution.

<Real>
Default = 1.7

GPSLOC

Controls where the grid point stresses are calculated for output to the .mnf file.

<Z1, Z2 and MID>
Default = Z1

GRDPNT

Obsolete NASTRAN parameter that will give information about the mass properties of the structure.

<GID>
Integer ≥ -1
Default = -1

GRIDFORM

Controls the output format of the .grid file.

<LONG, SHORT>
Default = SHORT

GYRO1D

Activates/deactivates the calculation of 1D Gyroscopic Matrix for 1D Rotors in Rotor dynamics.

<YES, NO>
Default = NO

GYROAVG

Used to select the frequency response analysis formulation type for rotor dynamics analysis.

<0, -1>
Default = 0

GYROTIMO

Controls the inclusion or exclusion of shear effect in the beam gyroscopic matrix.

<YES, NO>
Default = NO

HASHASSM

Enables hash-table based assembly.

<YES, NO>
Default = NO

HFREQ

Specifies the upper bound of the frequency range of interest for modal combination.

<Real>
Default = None

HFREQFL

Excludes modes with frequencies greater than HFREQFL in Coupled Modal Frequency Response Analysis (Acoustic Analysis).

<Real>
(Hertz)

Default = None

HGHCMPOK

Used to turn on or off the check for negative and very large compliance values.

<NO, YES>
Default = NO

I64SLV

Enforces the activation of internal long (64-bit) integer sparse direct solver.

<YES, NO>
Default = NO

INREL

Controls the calculation of inertia relief.

<0, -1, -2>
Default = 0, for static subcases
Default = -2, for modal frequency response subcases

ITAPE

Writes the ‘Tape Label’ at the beginning of the OUTPUT2 results file.

<-1, 0>
Default = -1

INTRFACE

Generates the .interface file to verify if proper connection has been established between the Fluid and Structure meshes at the interface.

<YES, NO>
Default = YES

K4CUTOFF

Sets cut-off value if the low rank representation for the structural damping matrix is selected.

<Real>
Default = 0.1

K4METH

Specifies the value of PARAM, LOWRANK, which indicates the solution type for the faster Modal Frequency Response solution method invoked by PARAM,FASTFR and the FastFRS interface invoked by PARAM,FFRS.

<-1.0, 0.0, 1.0>
Default = 1.0

KDAMP

Enters viscous modal damping into the stiffness matrix as structural damping.

<1, -1>
Default = 1

KGRGD

Include contributions from rigid elements in the geometric stiffness matrix.

<YES, NO>
Default = NO

KISSSOFT

Controls the creation of the condensed stiffness matrix in an ASCII file to be used by the KISSsoft program.

<YES, NO>
Default = NO

KTPLAST

Beneficial for problems involving a combination of plasticity, contact, and pretension

<1 < N < 10000>
No default

LFREQ

Used to remove the Rigid Body Modes from the Modal Space.

<Real>
Default = None

LFREQFL

Excludes modes with frequencies lower than LFREQFL in Coupled Modal Frequency Response Analysis (Acoustic Analysis).

<Real> (Hertz)
Default = None

LGDISP

Activates Large Displacement Nonlinear Analysis.

<1, 0, -1>
Default = 0

LMSOUT

Outputs the condensed Flex Body Modes, full Diagonal Mass Matrix, and modal stresses to the .op2 file.

<YES, NO, STRESS>
Default = NO

LOWRANK

This parameter is obsolete. Use PARAM, K4METH to control the value of LOWRANK.

<0, -1, 1>
Default = 0

MASSDMIG

For static condensation with ASET of a static loadcase, the reduced stiffness matrix [k] and load vector {p} are created.

<YES, NO>
Default = NO

MAXDAMP

Identifies the maximum number of residual vectors to be calculated.

<Integer>
Default = 400

MBDH3D

Choose the type of the results output to the .h3d file for MBD analyses.

<NODAL, MODAL, BOTH, NONE>
Default = BOTH

MBDREC

Creates small and large flexible body files during Component Mode Synthesis (CMS).

<YES, NO>
Default = NO

MDK4OPT

Controls the internal calculation of material damping when different material damping values (GE on MATx) are specified for different regions in a model.

<0, 1>
Default = 1

MEMTRIM

Activates/deactivates the memory-trim feature when using AMLS eigensolver.

<YES, NO>
Default = YES

MFILTER

Defines a threshold for the mode tracking matrix to check eigenvector correspondence.

<0.0 < real number < 1.0>

MODETRAK

Tracks mode numbers by comparing eigenvectors between iterations.

<-1, 0, 1, YES, NO>
Default = NO

NEGMASS

Allows run to proceed with negative diagonal mass terms.

<YES, NO>
Default = NO

NLFAT

Forces OptiStruct to run models in which fatigue solutions reference small displacement nonlinear analysis (NLSTAT) subcases.

This is not recommended; refer to the complete PARAM, NLFAT documentation for details.

<YES, NO>
Default = NO

NLMON

This parameter activates Nonlinear Results Monitoring. Currently, only displacement results monitoring is available.

<DISP, NO>

NPRBAR

Controls the number of the output INFORMATION #741 for RBAR element.

<Integer>
Default = 3

NPRBE2

Controls the number of the output INFORMATION #741 for RBE2 element.

<Integer>
Default = 3

NPRGDE

Controls the number of the output INFORMATION #742.

<Integer>
Default = 3

NUMEG

Specifies the anticipated number of modes to be calculated in order to estimate disk space usage.

<Integer>
Default = 1000

ODS

An Operating Deformed Shape (ODS) run requires the output for all the elements or all the grids for limited loading frequencies of interest.

<YES, NO>
Default = NO

OGEOM

Outputs model data to the OUTPUT2 results file.

<YES, NO>
Default = YES

OMACHPR

Selects newer version of certain OUTPUT2 datablocks.

<YES, NO>
Default = NO

OMID

Outputs stress and strain results for shell and membrane elements with reference to the material coordinate system.

<YES, NO>
Default =YES

OP2GM34

Controls the output of GEOM3 and GEOM4 data blocks to the .op2 file.

<TRUE, FALSE>
Default = TRUE

PBUSHT

Used to turn ON/OFF the usage of all PBUSHT Bulk Data Entries in the model.

<ON, OFF>
Default = ON

PBUSHTF

Specifies the reference frequency value for scaling factor lookup to update the nominal PBUSH Stiffness (K) values.

<Real>
No default

PELAST

Used to turn ON/OFF the usage of all PELAST Bulk Data Entries in the model.

<ON, OFF>
Default = ON

PLIGEXT

Prints the applied load vector in DMIG form to the .pligext file.

<YES, NO>
Default = NO

PNLSIZ

Increases the starting size of panel to the specified value

<Integer > 0 >

POST

Generates an OUTPUT2 results file.

<-1, -2, -5>

POSTEXT

Outputs the modal complex stiffness matrix and modal viscous damping matrix to the OUTPUT2 results file.

<YES, NO>
Default = NO

PRTDES

Controls the printing of Design Variables and Design Entities to the .out file.

<DVDP, DV, DP, NONE>
Default = DVDP

PRTRET

Controls the printing of Retained Response information to the .out file.

<ALL, NOSTR, NONE>
Default = ALL

PRESUBNL

Forces OptiStruct to run models in which Linear Buckling Analysis or Preloaded Analysis is defined, in conjunction with nonlinear materials (MATS1, MATHE, or MGASK) or Large Displacement Nonlinear Analysis.

This is not recommended. Refer to the complete PARAM, PRESUBNL documentation for details.

<YES, NO>
Default = NO

PRGPST

Outputs AutoSPC information to the .out file.

< YES, NO, ALL, NONE,< number of DOFs> >
Default = YES

PRINFACC

Controls the output of inertial relief rigid body forces and accelerations.

<1, 0>

RBE2FREE

Used to convert ERROR 725 into WARNING 825 when singular RBE2 elements are present in the model.

<YES, NO>
Default = NO

RBE3FREE

Used to convert ERROR 772 into WARNING 824 when free spiders on RBE3 elements are present in the model. These free spiders may contain singular degrees-of-freedom.

<YES, NO>
Default = NO

RBMEIG

Defines the cut-off eigenvalue for determining rigid body modes calculated by AMLS.

<Real>
Default = 0.1

REANAL

Reanalyze the final iteration of a topology optimization without penalization.

0.0 < Real < 1.0
No default

RECOVER

Allows you to request full-structure global mode shape output instead of the modes of the condensed system generated during Component Mode Synthesis (CMS).

<LB, UB>
Default for LB = 0.0, and UB must be specified

REFPNT

The reference point for Inertia Relief of the model.

<GEOM, CG>
Default = GEOM

RENUMOK

Allows you to correctly renumber the reversed (but acceptable) sequence of element grids without having to run (import and re-export) the model through HyperMesh.

<YES, NO, BLANK>
Default = YES

RFIOUT

Controls the output of modal super element for use in the RecurDyn multibody dynamics software from FunctionBay.

<YES, NO>
Default = NO

RHOCP

The scale factor used to calculate ERP in decibels (dB).

Real > 0.0
Default = 1.0

RICARDO

Controls the creation of the condensed flex body modes and full diagonal mass matrix to the .op2 file to be used by VALDYN from Ricardo Software.

<YES, NO>
Default = NO

RSPLICOR

RSPLINE end rotation correction.

<0, 1, REAL > 1.0>
Default = 0

S2K

Controls the creation of analysis results to be used by the STRENGTH2000 program to the .op2 file.

<YES, NO>
Default = NO

SEP1XOVR

The old and new location of moved shell grid points are printed if SEP1XOVR = 16.

<0, 16>
Default = 0

SEPLOT

Outputs display model to .seplot file, from a CMS run.

<YES, NO>
Default = YES

SHELOS11

Allows you to revert to the first order shell element formulation (for CQUAD4 and CTRIA3) used in version 11.0.240 and earlier.

<YES, NO>
Default = NO

SHL2MEM

A shell property (defined by the PSHELL bulk data entry) is automatically converted into a membrane property if the membrane thickness (field T) of the PSHELL bulk data entry is less than the value specified using PARAM, SHL2MEM.

<Real Number > 0.0>
No default

SHPBCKOR

Defines the type and order of approximation used in plate bending geometric stiffness for linear shell elements (CQUAD4, CTRIA3).

<1, 2>
Default = 1

SIMPACK

Requests generation of the SIMPACK .fbi file containing flexible body information for SIMPACK analysis.

<0, 1, 2, 3, 4>
Default = 0

SIMVER

This parameter can be used to select the SIMPACK version for multi-body dynamics analysis.

<8, 9>
Default = 9

SORTCON

Controls the output of violated constraints to the .out file from an optimization.

<Integer>
Default = 20

SPLC

Specifies the speed of sound used in the wave number and the complex particle velocity vector calculations.

Real > 0.0
Default = 1.0

SPLFAC

Specifies the scale factor (q) used to calculate the Sound Pressure Level in Radiated Sound Analysis.

Real > 0.0
Default = 1.0

SPLREFDB

Specifies the reference sound pressure value used to calculate the Sound Pressure Level (SPL) in decibels (dB).

Real > 0.0
Default = 1.0

SPLRHO

Specifies the density of the acoustic medium in the calculation of the complex acoustic sound pressure and the complex particle velocity vector.

Real > 0.0
Default = 1.0

SRCOMPS

Outputs the strength ratios for composite elements that have failure indices requested.

<YES, NO, or blank>
Default = NO

SS2GCR

Controls the accuracy of the external AMLS eigenvalue solution.

<Real>
Default = 5.0

STRTHR

Used to specify the von Mises stress threshold above which the stress results are output for a model.

<Real ≥ 0.0>
Default = 0.0

THCNTPEN

Controls the penalty factor used in thermal contact analysis.

<AUTO, LOW, HIGH>
Default = AUTO

TOLRSC

Connecting grid points of the shell element are moved onto the solid face.

<Real>
Default = 0.05

TRAKMETH

Used to select the criterion employed for mode tracking.

<0, 1, 2>
Default = 0

TRAKMTX

Controls output of the mode tracking matrix during optimization.

<0, 1>
Default = 0

TPS

Activates fast transient response analysis (only shell stress results output).

<YES, NO>
Default = YES

UCORD

Specifies the coordinate system in which the mass moment of inertia is output. It also can be used to control the point about which the mass moment of inertia is calculated.

<CID>
Integer ≥ -1
Default = -1

UHT

Outputs the UHT data block.

<YES, NO>
Default = NO

UNSYMSLV

Controls the inclusion or exclusion of non-symmetric terms in the tangent stiffness matrix due to friction in frictional contact problems.

<YES, NO>
Default = YES

VMOPT

Allows you to prevent the inclusion of the Virtual Mass Matrix in the Regular Mass Matrix for Modal Dynamic Subcases. In such cases, the virtual mass is added after the eigen solution and modes are modified based on the virtual mass matrix.

<Integer = 0, 1, 2>
Default = 0

W3

Converts structural damping to equivalent viscous damping for transient analysis.

<Real>
Default = 0.0

W4

Converts structural damping to equivalent viscous damping for transient analysis.

<Real>
Default = 0.0

WRH

Used to include or exclude frequency dependent hybrid damping in rotor dynamics analysis.

<Real>
Default = 0.0

WR3

Used to include or exclude frequency dependent damping in rotor dynamics analysis.

<Real>
Default = 0.0

WR4

Used to include or exclude frequency dependent damping in rotor dynamics analysis.

<Real>
Default = 0.0

WTMASS

Converts weights to masses using this multiplier.

<Real > 0.0>
Default = 1.0

XPOST

Used to create the .elfo (element forces), .elsh (element shear), and .endl (end loads) output files.

<YES, NO, NOFORCE>
Default = NO