Section#

The Section commands are used to create sections and profiles with their associated properties and behavior. The various section objects are all derived from the Section object. The various profile objects are all derived from the Profile object. See Property commands for the property assignment commands.

Objects in Section

Create sections#

In Mdb#

class SectionModel(name, description='', stefanBoltzmann=None, absoluteZero=None, waveFormulation=abaqusConstants.NOT_SET, modelType=abaqusConstants.STANDARD_EXPLICIT, universalGas=None, copyConstraints=ON, copyConnectors=ON, copyInteractions=ON)[source]#

Abaqus creates a Model object named Model-1 when a session is started.

Note

This object can be accessed by:

mdb.models[name]

Note

Check SectionModel on help.3ds.com/0.1..

Public Data Attributes:

Inherited from ModelBase

name

A String specifying the repository key.

stefanBoltzmann

None or a Float specifying the Stefan-Boltzmann constant.

absoluteZero

None or a Float specifying the absolute zero constant.

waveFormulation

A SymbolicConstant specifying the type of incident wave formulation to be used in acoustic problems.

universalGas

None or a Float specifying the universal gas constant.

noPartsInputFile

A Boolean specifying whether an input file should be written without parts and assemblies.

restartIncrement

An Int specifying the increment, interval, iteration or cycle where the restart analysis will start.

endRestartStep

A Boolean specifying that the step specified by restartStep should be terminated at the increment specified by restartIncrement.

shellToSolid

A Boolean specifying that a shell global model drives a solid submodel.

lastChangedCount

A Float specifying the time stamp that indicates when the model was last changed.

description

A String specifying the purpose and contents of the Model object.

restartJob

A String specifying the name of the job that generated the restart data.

restartStep

A String specifying the name of the step where the restart analysis will start.

globalJob

A String specifying the name of the job that generated the results for the global model.

copyConstraints

A boolean specifying the status of constraints created in a model, in the model which instances this model.

copyConnectors

A boolean specifying the status of connectors created in a model, in the model which instances this model.

copyInteractions

A boolean specifying the status of interactions created in a model, in the model which instances this model.

keywordBlock

A KeywordBlock object.

rootAssembly

An Assembly object.

amplitudes

A repository of Amplitude objects.

profiles

A repository of Profile objects.

boundaryConditions

A repository of BoundaryCondition objects.

constraints

A repository of ConstrainedSketchConstraint objects.

analyticalFields

A repository of AnalyticalField objects.

discreteFields

A repository of DiscreteField objects.

predefinedFields

A repository of PredefinedField objects.

interactions

A repository of Interaction objects.

interactionProperties

A repository of InteractionProperty objects.

contactControls

A repository of ContactControl objects.

contactInitializations

A repository of ContactInitialization objects.

contactStabilizations

A repository of ContactStabilization objects.

linkedInstances

A tuple of tuples of Strings specifying the linked child PartInstance name in the current model to the corresponding parent PartInstance name in a different model.

linkedParts

A tuple of tuples of Strings specifying the linked child Part name in the current model to the corresponding parent Part name in a different model.

loads

A repository of Load objects.

materials

A repository of Material objects.

calibrations

A repository of Calibration objects.

sections

A repository of Section objects.

remeshingRules

A repository of RemeshingRule objects.

sketches

A repository of ConstrainedSketch objects.

parts

A repository of Part objects.

steps

A repository of Step objects.

featureOptions

A FeatureOptions object.

adaptiveMeshConstraints

A repository of AdaptiveMeshConstraint objects.

adaptiveMeshControls

A repository of AdaptiveMeshControl objects.

timePoints

A repository of TimePoint objects.

filters

A repository of Filter objects.

integratedOutputSections

A repository of IntegratedOutputSection objects.

fieldOutputRequests

A repository of FieldOutputRequest objects.

historyOutputRequests

A repository of HistoryOutputRequest objects.

optimizationTasks

A repository of OptimizationTask objects.

tableCollections

A repository of TableCollection objects.

eventSeriesTypes

A repository of EventSeriesType objects.

eventSeriesDatas

A repository of EventSeriesData objects.

Public Methods:

AcousticInfiniteSection(name, material[, ...])

This method creates an AcousticInfiniteSection object.

AcousticInterfaceSection(name[, thickness])

This method creates an AcousticInterfaceSection object.

BeamSection(name, integration, profile[, ...])

This method creates a BeamSection object.

CohesiveSection(name, response, material[, ...])

This method creates a CohesiveSection object.

CompositeShellSection(name, layup[, ...])

This method creates a CompositeShellSection object.

CompositeSolidSection(name, layup[, ...])

This method creates a CompositeSolidSection object.

ConnectorSection(name[, assembledType, ...])

This method creates a ConnectorSection object.

EulerianSection(name, data)

This method creates a EulerianSection object.

GasketSection(name, material[, ...])

This method creates a GasketSection object.

GeneralStiffnessSection(name, stiffnessMatrix)

This method creates a GeneralStiffnessSection object.

HomogeneousShellSection(name, material[, ...])

This method creates a HomogeneousShellSection object.

HomogeneousSolidSection(name, material[, ...])

This method creates a HomogeneousSolidSection object.

MembraneSection(name, material[, thickness, ...])

This method creates a MembraneSection object.

MPCSection(name, mpcType[, userMode, userType])

This method creates a MPCSection object.

PEGSection(name, material[, thickness, ...])

This method creates a PEGSection object.

SurfaceSection(name[, useDensity, density])

This method creates a SurfaceSection object.

TrussSection(name, material[, area])

This method creates a TrussSection object.
Inherited from ModelBase

__init__(name[, description, ...])

This method creates a Model object.

ModelFromInputFile(name, inputFileName)

This method creates a Model object by reading the keywords in an input file and creating the corresponding Abaqus/CAE objects.

ModelFromOdbFile(name, odbFileName)

This method creates a Model object by reading an output database and creating any corresponding Abaqus/CAE objects.

ModelFromNastranFile(modelName, inputFileName)

This method creates a Model object by reading the keywords in a Nastran bulk data file or Nastran input file and creating any corresponding Abaqus/CAE objects.

setValues([description, noPartsInputFile, ...])

This method modifies the Model object.
AcousticInfiniteSection(name, material, thickness=1, order=10)[source]#

This method creates an AcousticInfiniteSection object.

Note

This function can be accessed by:

mdb.models[name].AcousticInfiniteSection
session.odbs[name].AcousticInfiniteSection

Note

Check AcousticInfiniteSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • material (str) – A String specifying the name of the material.

  • thickness (float, default: 1) – A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

  • order (int, default: 10) – An Int specifying the number of ninth-order polynomials that will be used to resolve the variation of the acoustic field in the infinite direction. Possible values are 0 << order ≤ 10. The default value is 10.

Returns:

An AcousticInfiniteSection object.

Return type:

AcousticInfiniteSection

Raises:

  • InvalidNameError –

  • RangeError –

AcousticInterfaceSection(name, thickness=1)[source]#

This method creates an AcousticInterfaceSection object.

Note

This function can be accessed by:

mdb.models[name].AcousticInterfaceSection
session.odbs[name].AcousticInterfaceSection

Note

Check AcousticInterfaceSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • thickness (float, default: 1) – A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

Returns:

An AcousticInterfaceSection object.

Return type:

AcousticInterfaceSection

Raises:

  • InvalidNameError –

  • RangeError –

BeamSection(name, integration, profile, poissonRatio=0, thermalExpansion=OFF, temperatureDependency=OFF, dependencies=0, density=None, referenceTemperature=None, temperatureVar=abaqusConstants.LINEAR, alphaDamping=0, betaDamping=0, compositeDamping=0, useFluidInertia=OFF, submerged=abaqusConstants.FULLY, fluidMassDensity=None, crossSectionRadius=None, lateralMassCoef=1, axialMassCoef=0, massOffsetX=0, massOffsetY=0, beamShape=abaqusConstants.CONSTANT, material='', table=(), outputPts=(), centroid=(0.0, 0.0), shearCenter=(0.0, 0.0), profileEnd='')[source]#

This method creates a BeamSection object.

Note

This function can be accessed by:

mdb.models[name].BeamSection
session.odbs[name].BeamSection

Note

Check BeamSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • integration (Literal[BEFORE_ANALYSIS, DURING_ANALYSIS]) – A SymbolicConstant specifying the integration method for the section. Possible values are BEFORE_ANALYSIS and DURING_ANALYSIS.

  • profile (str) – A String specifying the name of the profile. This argument represents the start profile in case of beamShape = TAPERED.

  • poissonRatio (float, default: 0) – A Float specifying the Poisson’s ratio of the section. The default value is 0.0.

  • thermalExpansion (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether to use thermal expansion data. The default value is OFF.

  • temperatureDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the data depend on temperature. The default value is OFF.

  • dependencies (int, default: 0) – An Int specifying the number of field variable dependencies. The default value is 0.

  • density (Optional[float], default: None) – None or a Float specifying the density of the section. The default value is None.

  • referenceTemperature (Optional[float], default: None) – None or a Float specifying the reference temperature of the section. The default value is None.

  • temperatureVar (Literal[LINEAR, INTERPOLATED], default: LINEAR) – A SymbolicConstant specifying the temperature variation for the section. Possible values are LINEAR and INTERPOLATED. The default value is LINEAR.

  • alphaDamping (float, default: 0) – A Float specifying the αRαR factor to create mass proportional damping in direct-integration dynamics. The default value is 0.0.

  • betaDamping (float, default: 0) – A Float specifying the βRβR factor to create stiffness proportional damping in direct-integration dynamics. The default value is 0.0.

  • compositeDamping (float, default: 0) – A Float specifying the fraction of critical damping to be used in calculating composite damping factors for the modes (for use in modal dynamics). The default value is 0.0.

  • useFluidInertia (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether added mass effects will be simulated. The default value is OFF.

  • submerged (Literal[FULLY, HALF], default: FULLY) – A SymbolicConstant specifying whether the section is either full submerged or half submerged. This argument applies only when useFluidInertia = True. Possible values are FULLY and HALF. The default value is FULLY.

  • fluidMassDensity (Optional[float], default: None) – None or a Float specifying the mass density of the fluid. This argument applies only when useFluidInertia = True and must be specified in that case. The default value is None.

  • crossSectionRadius (Optional[float], default: None) – None or a Float specifying the radius of the cylindrical cross-section. This argument applies only when useFluidInertia = True and must be specified in that case. The default value is None.

  • lateralMassCoef (float, default: 1) – A Float specifying the added mass coefficient, CACA, for lateral motions of the beam. This argument applies only when*useFluidInertia* = True. The default value is 1.0.

  • axialMassCoef (float, default: 0) – A Float specifying the added mass coefficient, C(A−E)C(A-E), for motions along the axis of the beam. This argument affects only the term added to the free end(s) of the beam, and applies only when useFluidInertia = True. The default value is 0.0.

  • massOffsetX (float, default: 0) – A Float specifying the local 1-coordinate of the center of the cylindrical cross-section with respect to the beam cross-section. This argument applies only when useFluidInertia = True. The default value is 0.0.

  • massOffsetY (float, default: 0) – A Float specifying the local 2-coordinate of the center of the cylindrical cross-section with respect to the beam cross-section. This argument applies only when useFluidInertia = True. The default value is 0.0.

  • beamShape (Literal[CONSTANT, TAPERED], default: CONSTANT) – A SymbolicConstant specifying the change in cross-section of the beam along length. Possible values are CONSTANT and TAPERED. The default value is CONSTANT. This parameter is available for manipulating the model database but not for the ODB API.

  • material (str, default: '') – A String specifying the name of the material. The default value is an empty string. The material is required when integration is “DURING_ANALYSIS”.

  • table (tuple, default: ()) – A sequence of sequences of Floats specifying the items described below. The default value is an empty sequence.

  • outputPts (tuple, default: ()) – A sequence of pairs of Floats specifying the positions at which output is requested. The default value is an empty sequence.

  • centroid (Tuple[float, float], default: (0.0, 0.0)) – A pair of Floats specifying the X - Y coordinates of the centroid. The default value is (0.0, 0.0).

  • shearCenter (Tuple[float, float], default: (0.0, 0.0)) – A pair of Floats specifying the X - Y coordinates of the shear center. The default value is (0.0, 0.0).

  • profileEnd (str, default: '') – A String specifying the name of the end profile. The type of the end profile must be same as that of the start profile. This argument is valid only when beamShape = TAPERED. The default value is an empty string. This parameter is available for manipulating the model database but not for the ODB API.

Returns:

A BeamSection object.

Return type:

BeamSection

CohesiveSection(name, response, material, initialThicknessType=abaqusConstants.SOLVER_DEFAULT, initialThickness=1, outOfPlaneThickness=None)[source]#

This method creates a CohesiveSection object.

Note

This function can be accessed by:

mdb.models[name].CohesiveSection
session.odbs[name].CohesiveSection

Note

Check CohesiveSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • response (Literal[TRACTION_SEPARATION, CONTINUUM, GASKET]) – A SymbolicConstant specifying the geometric assumption that defines the constitutive behavior of the cohesive elements. Possible values are TRACTION_SEPARATION, CONTINUUM, and GASKET.

  • material (str) – A String specifying the name of the material.

  • initialThicknessType (Literal[SOLVER_DEFAULT, SPECIFY], default: SOLVER_DEFAULT) – A SymbolicConstant specifying the method used to compute the initial thickness. Possible values are:SOLVER_DEFAULT, specifying that Abaqus will use the analysis product defaultGEOMETRY, specifying that Abaqus will compute the thickness from the nodal coordinates of the elements.SPECIFY, specifying that Abaqus will use the value given for initialThickness The default value is SOLVER_DEFAULT.

  • initialThickness (float, default: 1) – A Float specifying the initial thickness for the section. The initialThickness argument applies only when initialThicknessType = SPECIFY. The default value is 1.0.

  • outOfPlaneThickness (Optional[float], default: None) – None or a Float specifying the out-of-plane thickness for the section. The default value is None.

Returns:

A CohesiveSection object.

Return type:

CohesiveSection

Raises:

RangeError –

CompositeShellSection(name, layup, symmetric=OFF, thicknessType=abaqusConstants.UNIFORM, preIntegrate=OFF, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, integrationRule=abaqusConstants.SIMPSON, temperature=abaqusConstants.GRADIENT, idealization=abaqusConstants.NO_IDEALIZATION, nTemp=None, thicknessModulus=None, useDensity=OFF, density=0, layupName='', thicknessField='', nodalThicknessField='')[source]#

This method creates a CompositeShellSection object.

Note

This function can be accessed by:

mdb.models[name].parts[name].compositeLayups[i].CompositeShellSection
mdb.models[name].CompositeShellSection
session.odbs[name].CompositeShellSection

Note

Check CompositeShellSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • layup (List[SectionLayer]) – A SectionLayerArray object specifying the shell cross-section.

  • symmetric (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.

  • thicknessType (Literal[UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, NODAL_DISCRETE_FIELD], default: UNIFORM) – A SymbolicConstant specifying the distribution used for defining the thickness of the elements. Possible values are UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, and NODAL_DISCRETE_FIELD. The default value is UNIFORM.

  • preIntegrate (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the shell section properties are specified by the user prior to the analysis (ON) or integrated during the analysis (OFF). The default value is OFF.

  • poissonDefinition (Literal[DEFAULT, VALUE], default: DEFAULT) – A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

  • poisson (float, default: 0) – A Float specifying the Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

  • integrationRule (Literal[SIMPSON, GAUSS], default: SIMPSON) – A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.

  • temperature (Literal[GRADIENT, POINTWISE], default: GRADIENT) – A SymbolicConstant specifying the mode used for temperature and field variable input across the section thickness. Possible values are GRADIENT and POINTWISE. The default value is GRADIENT.

  • idealization (Literal[NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, BENDING], default: NO_IDEALIZATION) – A SymbolicConstant specifying the mechanical idealization used for the section calculations. This member is only applicable when preIntegrate is set to ON. Possible values are NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, and BENDING. The default value is NO_IDEALIZATION.

  • nTemp (Optional[int], default: None) – None or an Int specifying the number of temperature points to be input. This argument is valid only when temperature = POINTWISE. The default value is None.

  • thicknessModulus (Optional[float], default: None) – None or a Float specifying the effective thickness modulus. This argument is relevant only for continuum shells and must be used in conjunction with the argument poisson. The default value is None.

  • useDensity (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not to use the value of density. The default value is OFF.

  • density (float, default: 0) – A Float specifying the value of density to apply to this section. The default value is 0.0.

  • layupName (str, default: '') – A String specifying the layup name for this section. The default value is an empty string.

  • thicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements. The thicknessField argument applies only when thicknessType = ANALYTICAL_FIELD or thicknessType = DISCRETE_FIELD. The default value is an empty string.

  • nodalThicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements at each node. The nodalThicknessField argument applies only when thicknessType = NODAL_ANALYTICAL_FIELD or thicknessType = NODAL_DISCRETE_FIELD. The default value is an empty string.

Returns:

A CompositeShellSection object.

Return type:

CompositeShellSection

CompositeSolidSection(name, layup, symmetric=OFF, layupName='')[source]#

This method creates a CompositeSolidSection object.

Note

This function can be accessed by:

mdb.models[name].CompositeSolidSection
session.odbs[name].CompositeSolidSection

Note

Check CompositeSolidSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • layup (List[SectionLayer]) – A SectionLayerArray object specifying the solid cross-section.

  • symmetric (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.

  • layupName (str, default: '') – A String specifying the layup name for this section. The default value is an empty string.

Returns:

A CompositeSolidSection object.

Return type:

CompositeSolidSection

ConnectorSection(name, assembledType=abaqusConstants.NONE, rotationalType=abaqusConstants.NONE, translationalType=abaqusConstants.NONE, integration=abaqusConstants.UNSPECIFIED, u1ReferenceLength=None, u2ReferenceLength=None, u3ReferenceLength=None, ur1ReferenceAngle=None, ur2ReferenceAngle=None, ur3ReferenceAngle=None, massPerLength=None, contactAngle=None, materialFlowFactor=1.0, regularize=ON, defaultTolerance=ON, regularization=0.03, extrapolation=abaqusConstants.CONSTANT, behaviorOptions=Ellipsis)[source]#

This method creates a ConnectorSection object.

Note

This function can be accessed by:

mdb.models[name].ConnectorSection
session.odbs[name].ConnectorSection

Note

Check ConnectorSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • assembledType (Literal[NONE, BEAM, BUSHING, CVJOINT, CYLINDRICAL, HINGE, PLANAR, RETRACTOR, SLIPRING, TRANSLATOR, UJOINT, WELD], default: NONE) – A SymbolicConstant specifying the assembled connection type. Possible values are:NONEBEAMBUSHINGCVJOINTCYLINDRICALHINGEPLANARRETRACTORSLIPRINGTRANSLATORUJOINTWELDThe default value is NONE.You cannot include the assembledType argument if translationalType or rotationalType are given a value other than NONE. At least one of the arguments assembledType, translationalType, or rotationalType must be given a value other than NONE.

  • rotationalType (Literal[NONE, ALIGN, CARDAN, CONSTANT_VELOCITY, EULER, FLEXION_TORSION, FLOW_CONVERTER, PROJECTION_FLEXION_TORSION, REVOLUTE, ROTATION, ROTATION_ACCELEROMETER, UNIVERSAL], default: NONE) – A SymbolicConstant specifying the basic rotational connection type. Possible values are:NONEALIGNCARDANCONSTANT_VELOCITYEULERFLEXION_TORSIONFLOW_CONVERTERPROJECTION_FLEXION_TORSIONREVOLUTEROTATIONROTATION_ACCELEROMETERUNIVERSALThe default value is NONE.You cannot include the rotationalType argument if assembledType is given a value other than NONE. At least one of the arguments assembledType, translationalType, or rotationalType must be given an value other than NONE.

  • translationalType (Literal[NONE, ACCELEROMETER, AXIAL, CARTESIAN, JOIN, LINK, PROJECTION_CARTESIAN, RADIAL_THRUST, SLIDE_PLANE, SLOT], default: NONE) – A SymbolicConstant specifying the basic translational connection type. Possible values are:NONEACCELEROMETERAXIALCARTESIANJOINLINKPROJECTION_CARTESIANRADIAL_THRUSTSLIDE_PLANESLOTThe default value is NONE.You cannot include the translationalType argument if assembledType is given a value other than NONE. At least one of the arguments assembledType, translationalType, or rotationalType must be given an value other than NONE.

  • integration (Literal[UNSPECIFIED, IMPLICIT, EXPLICIT], default: UNSPECIFIED) – A SymbolicConstant specifying the time integration scheme to use for analysis. This argument is applicable only to an Abaqus/Explicit analysis. Possible values are UNSPECIFIED, IMPLICIT, and EXPLICIT. The default value is UNSPECIFIED.

  • u1ReferenceLength (Optional[float], default: None) – None or a Float specifying the reference length associated with constitutive response for the first component of relative motion. The default value is None.

  • u2ReferenceLength (Optional[float], default: None) – None or a Float specifying the reference length associated with constitutive response for the second component of relative motion. The default value is None.

  • u3ReferenceLength (Optional[float], default: None) – None or a Float specifying the reference length associated with constitutive response for the third component of relative motion. The default value is None.

  • ur1ReferenceAngle (Optional[float], default: None) – None or a Float specifying the reference angle in degrees associated with constitutive response for the fourth component of relative motion. The default value is None.

  • ur2ReferenceAngle (Optional[float], default: None) – None or a Float specifying the reference angle in degrees associated with constitutive response for the fifth component of relative motion. The default value is None.

  • ur3ReferenceAngle (Optional[float], default: None) – None or a Float specifying the reference angle in degrees associated with constitutive response for the sixth component of relative motion. The default value is None.

  • massPerLength (Optional[float], default: None) – None or a Float specifying the mass per unit reference length of belt material. This argument is applicable only when assembledType = SLIPRING, and must be specified in that case. The default value is None.

  • contactAngle (Optional[float], default: None) – None or a Float specifying the contact angle made by the belt wrapping around node b. This argument is applicable only to an Abaqus/Explicit analysis, and only when assembledType = SLIPRING. The default value is None.

  • materialFlowFactor (float, default: 1.0) – A Float specifying the scaling factor for material flow at node b. This argument is applicable only when assembledType = RETRACTOR or rotationalType = FLOW_CONVERTER. The default value is 1.0.

  • regularize (Union[AbaqusBoolean, bool], default: ON) – A Boolean specifying whether or not all tabular data associated with the behaviorOptions will be regularized. This argument is applicable only for an Abaqus/Explicit analysis. The default value is ON.

  • defaultTolerance (Union[AbaqusBoolean, bool], default: ON) – A Boolean specifying whether or not the default regularization tolerance will be used for all tabular data associated with the behaviorOptions. This argument is applicable only for an Abaqus/Explicit analysis and only if regularize = ON. The default value is ON.

  • regularization (float, default: 0.03) – A Float specifying the regularization increment to be used for all tabular data associated with the behaviorOptions. This argument is applicable only for an Abaqus/Explicit analysis and only if regularize = ON and defaultTolerance = OFF. The default value is 0.03.

  • extrapolation (Literal[CONSTANT, LINEAR], default: CONSTANT) – A SymbolicConstant specifying the extrapolation technique to be used for all tabular data associated with the behaviorOptions. Possible values are CONSTANT and LINEAR. The default value is CONSTANT.

  • behaviorOptions (List[ConnectorBehaviorOption], default: Ellipsis) – A ConnectorBehaviorOptionArray object.

Returns:

A ConnectorSection object.

Return type:

ConnectorSection

Raises:

  • InvalidNameError –

  • RangeError –

EulerianSection(name, data)[source]#

This method creates a EulerianSection object.

Note

This function can be accessed by:

mdb.models[name].EulerianSection
session.odbs[name].EulerianSection

Note

Check EulerianSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • data (str) – A String-to-String Dictionary specifying a dictionary mapping Material instance names to Material names. Internally the specified mapping gets sorted on Material instance name.

Returns:

An EulerianSection object.

Return type:

EulerianSection

GasketSection(name, material, crossSection=1, initialGap=0, initialThickness=abaqusConstants.DEFAULT, initialVoid=0, stabilizationStiffness=abaqusConstants.DEFAULT)[source]#

This method creates a GasketSection object.

Note

This function can be accessed by:

mdb.models[name].GasketSection
session.odbs[name].GasketSection

Note

Check GasketSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • material (str) – A String specifying the name of the material of which the gasket is made or material that defines gasket behavior.

  • crossSection (float, default: 1) – A Float specifying the cross-sectional area, width, or out-of-plane thickness, if applicable, depending on the gasket element type. The default value is 1.0.

  • initialGap (float, default: 0) – A Float specifying the initial gap. The default value is 0.0.

  • initialThickness (Union[Literal[DEFAULT], float], default: DEFAULT) – The SymbolicConstant DEFAULT or a Float specifying the initial gasket thickness. If DEFAULT is specified, the initial thickness is determined using nodal coordinates. The default value is DEFAULT.

  • initialVoid (float, default: 0) – A Float specifying the initial void. The default value is 0.0.

  • stabilizationStiffness (Union[Literal[DEFAULT], float], default: DEFAULT) – The SymbolicConstant DEFAULT or a Float specifying the default stabilization stiffness used in all but link elements to stabilize gasket elements that are not supported at all nodes, such as those that extend outside neighboring components. If DEFAULT is specified, a value is used equal to 10-9 times the initial compressive stiffness in the thickness direction. The default value is DEFAULT.

Returns:

A GasketSection object. and ValueError.

Return type:

GasketSection

GeneralStiffnessSection(name, stiffnessMatrix, referenceTemperature=None, applyThermalStress=OFF, temperatureDependency=OFF, dependencies=0, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, useDensity=OFF, density=0, thermalStresses=(), scalingData=())[source]#

This method creates a GeneralStiffnessSection object.

Note

This function can be accessed by:

mdb.models[name].GeneralStiffnessSection
session.odbs[name].GeneralStiffnessSection

Note

Check GeneralStiffnessSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • stiffnessMatrix (tuple) – A sequence of Floats specifying the stiffness matrix for the section in the order D11, D12, D22, D13, D23, D33, …., D66. Twenty-one entries must be given.

  • referenceTemperature (Optional[float], default: None) – None or a Float specifying the reference temperature for thermal expansion. The default value is None.

  • applyThermalStress (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not the section stiffness varies with thermal stresses. The default value is OFF.

  • temperatureDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the data depend on temperature. The default value is OFF.

  • dependencies (int, default: 0) – An Int specifying the number of field variable dependencies. The default value is 0.

  • poissonDefinition (Literal[VALUE, DEFAULT], default: DEFAULT) – A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

  • poisson (float, default: 0) – A Float specifying the Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

  • useDensity (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not to use the value of density. The default value is OFF.

  • density (float, default: 0) – A Float specifying the value of density to apply to this section. The default value is 0.0.

  • thermalStresses (tuple, default: ()) – A sequence of Floats specifying the generalized stress values caused by a unit temperature rise. Six entries must be given if the value of applyThermalStress is set to True. The default value is (“”).

  • scalingData (tuple, default: ()) – A sequence of sequences of Floats specifying the scaling factors for given temperatures and/or field data. Each row should contain (Y, alpha, T, F1,…,Fn). The default value is an empty sequence.

Returns:

A GeneralStiffnessSection object.

Return type:

GeneralStiffnessSection

HomogeneousShellSection(name, material, thickness=0, numIntPts=5, thicknessType=abaqusConstants.UNIFORM, preIntegrate=OFF, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, integrationRule=abaqusConstants.SIMPSON, temperature=abaqusConstants.GRADIENT, idealization=abaqusConstants.NO_IDEALIZATION, nTemp=None, thicknessModulus=None, useDensity=OFF, density=0, thicknessField='', nodalThicknessField='')[source]#

This method creates a HomogeneousShellSection object.

Note

This function can be accessed by:

mdb.models[name].parts[name].compositeLayups[i].HomogeneousShellSection
mdb.models[name].HomogeneousShellSection
session.odbs[name].HomogeneousShellSection

Note

Check HomogeneousShellSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • material (str) – A String specifying the name of the section material.

  • thickness (float, default: 0) – A Float specifying the thickness of the section. The thickness argument applies only when thicknessType = UNIFORM. The default value is 0.0.

  • numIntPts (int, default: 5) – An Int specifying the number of integration points to be used through the section. Possible values are numIntPts >> 0. The default value is 5.To use the default settings of the analysis products, set numIntPts to 5 if integrationRule = SIMPSON or set numIntPts to 7 if integrationRule = GAUSS.

  • thicknessType (Literal[UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, NODAL_DISCRETE_FIELD], default: UNIFORM) – A SymbolicConstant specifying the distribution used for defining the thickness of the elements. Possible values are UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, and NODAL_DISCRETE_FIELD. The default value is UNIFORM.

  • preIntegrate (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the shell section properties are specified by the user prior to the analysis (ON) or integrated during the analysis (OFF). The default value is OFF.

  • poissonDefinition (Literal[DEFAULT, VALUE], default: DEFAULT) – A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

  • poisson (float, default: 0) – A Float specifying the Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

  • integrationRule (Literal[SIMPSON, GAUSS], default: SIMPSON) – A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.

  • temperature (Literal[GRADIENT, POINTWISE], default: GRADIENT) – A SymbolicConstant specifying the mode used for temperature and field variable input across the section thickness. Possible values are GRADIENT and POINTWISE. The default value is GRADIENT.

  • idealization (Literal[NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, BENDING], default: NO_IDEALIZATION) – A SymbolicConstant specifying the mechanical idealization used for the section calculations. This member is only applicable when preIntegrate is set to ON. Possible values are NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, and BENDING. The default value is NO_IDEALIZATION.

  • nTemp (Optional[int], default: None) – None or an Int specifying the number of temperature points to be input. This argument is valid only when temperature = POINTWISE. The default value is None.

  • thicknessModulus (Optional[float], default: None) – None or a Float specifying the effective thickness modulus. This argument is relevant only for continuum shells and must be used in conjunction with the argument poisson. The default value is None.

  • useDensity (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not to use the value of density. The default value is OFF.

  • density (float, default: 0) – A Float specifying the value of density to apply to this section. The default value is 0.0.

  • thicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements. The thicknessField argument applies only when thicknessType = ANALYTICAL_FIELD or thicknessType = DISCRETE_FIELD. The default value is an empty string.

  • nodalThicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements at each node. The nodalThicknessField argument applies only when thicknessType = NODAL_ANALYTICAL_FIELD or thicknessType = NODAL_DISCRETE_FIELD. The default value is an empty string.

Returns:

A HomogeneousShellSection object.

Return type:

HomogeneousShellSection

HomogeneousSolidSection(name, material, thickness=1.0)[source]#

This method creates a HomogeneousSolidSection object.

Note

This function can be accessed by:

mdb.models[name].HomogeneousSolidSection
session.odbs[name].HomogeneousSolidSection

Note

Check HomogeneousSolidSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • material (str) – A String specifying the name of the material.

  • thickness (float, default: 1.0) –

    A Float specifying the thickness of the section. Possible values are None or greater than zero. The default value is 1.0.

    Changed in version 2018: The default value is now 1.0 instead of None.

Returns:

A HomogeneousSolidSection object.

Return type:

HomogeneousSolidSection

Raises:

  • InvalidNameError –

  • RangeError –

MPCSection(name, mpcType, userMode=abaqusConstants.DOF_MODE, userType=0)[source]#

This method creates a MPCSection object.

Note

This function can be accessed by:

mdb.models[name].MPCSection
session.odbs[name].MPCSection

Note

Check MPCSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • mpcType (Literal[BEAM_MPC, ELBOW_MPC, PIN_MPC, LINK_MPC, TIE_MPC, USER_DEFINED]) – A SymbolicConstant specifying the MPC type of the section. Possible values are BEAM_MPC, ELBOW_MPC, PIN_MPC, LINK_MPC, TIE_MPC, and USER_DEFINED.

  • userMode (Literal[DOF_MODE, NODE_MODE], default: DOF_MODE) – A SymbolicConstant specifying the mode of the MPC when it is user-defined. Possible values are DOF_MODE and NODE_MODE. The default value is DOF_MODE.The userMode argument applies only when mpcType = USER_DEFINED.

  • userType (int, default: 0) – An Int specifying to differentiate between different constraint types in a user-defined MPCSection. The default value is 0.The userType argument applies only when mpcType = USER_DEFINED.

Returns:

A MPCSection object.

Return type:

MPCSection

Raises:

RangeError –

MembraneSection(name, material, thickness=1, thicknessType=abaqusConstants.UNIFORM, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, thicknessField='')[source]#

This method creates a MembraneSection object.

Note

This function can be accessed by:

mdb.models[name].MembraneSection
session.odbs[name].MembraneSection

Note

Check MembraneSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • material (str) – A String specifying the name of the material.

  • thickness (float, default: 1) – A Float specifying the thickness for the section. Possible values are thickness >> 0.0. The default value is 1.0.

  • thicknessType (Literal[UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD], default: UNIFORM) – A SymbolicConstant specifying the distribution used for defining the thickness of the elements. Possible values are UNIFORM, ANALYTICAL_FIELD, and DISCRETE_FIELD. The default value is UNIFORM.

  • poissonDefinition (Literal[DEFAULT, VALUE], default: DEFAULT) – A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

  • poisson (float, default: 0) – A Float specifying the section Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

  • thicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements. The thicknessField argument applies only when thicknessType = ANALYTICAL_FIELD or thicknessType = DISCRETE_FIELD. The default value is an empty string.

Returns:

A MembraneSection object.

Return type:

MembraneSection

Raises:

RangeError –

PEGSection(name, material, thickness=1, wedgeAngle1=0, wedgeAngle2=0)[source]#

This method creates a PEGSection object.

Note

This function can be accessed by:

mdb.models[name].PEGSection
session.odbs[name].PEGSection

Note

Check PEGSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • material (str) – A String specifying the name of the material.

  • thickness (float, default: 1) – A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

  • wedgeAngle1 (float, default: 0) – A Float specifying the value of the x component of the angle between the bounding planes, ΔϕxΔ⁢ϕx. The default value is 0.0.

  • wedgeAngle2 (float, default: 0) – A Float specifying the value of the y component of the angle between the bounding planes, ΔϕyΔ⁢ϕy. The default value is 0.0.

Returns:

A PEGSection object.

Return type:

PEGSection

Raises:

  • InvalidNameError –

  • RangeError –

SurfaceSection(name, useDensity=OFF, density=0)[source]#

This method creates a SurfaceSection object.

Note

This function can be accessed by:

mdb.models[name].SurfaceSection
session.odbs[name].SurfaceSection

Note

Check SurfaceSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • useDensity (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not to use the value of density. The default value is OFF.

  • density (float, default: 0) – A Float specifying the value of density to apply to this section. The default value is 0.0.

Returns:

A SurfaceSection object.

Return type:

SurfaceSection

Raises:

RangeError –

TrussSection(name, material, area=1)[source]#

This method creates a TrussSection object.

Note

This function can be accessed by:

mdb.models[name].TrussSection
session.odbs[name].TrussSection

Note

Check TrussSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • material (str) – A String specifying the name of the material.

  • area (float, default: 1) – A Float specifying the cross-sectional area for the section. Possible values are area >> 0. The default value is 1.0.

Returns:

A TrussSection object.

Return type:

TrussSection

Raises:

RangeError –

In Odb#

class SectionOdb(name, analysisTitle='', description='', path='')[source]#

Public Data Attributes:

Inherited from OdbBase

isReadOnly

A Boolean specifying whether the output database was opened with read-only access.

amplitudes

A repository of Amplitude objects.

filters

A repository of Filter objects.

rootAssembly

An OdbAssembly object.

jobData

A JobData object.

parts

A repository of OdbPart objects.

materials

A repository of Material objects.

steps

A repository of OdbStep objects.

sections

A repository of Section objects.

sectionCategories

A repository of SectionCategory objects.

sectorDefinition

A SectorDefinition object.

userData

A UserData object.

customData

A RepositorySupport object.

profiles

A repository of Profile objects.

Public Methods:

AcousticInfiniteSection(name, material[, ...])

This method creates an AcousticInfiniteSection object.

AcousticInterfaceSection(name[, thickness])

This method creates an AcousticInterfaceSection object.

BeamSection(name, integration, profile[, ...])

This method creates a BeamSection object.

CohesiveSection(name, response, material[, ...])

This method creates a CohesiveSection object.

CompositeShellSection(name, layup[, ...])

This method creates a CompositeShellSection object.

CompositeSolidSection(name, layup[, ...])

This method creates a CompositeSolidSection object.

ConnectorSection(name[, assembledType, ...])

This method creates a ConnectorSection object.

EulerianSection(name, data)

This method creates a EulerianSection object.

GasketSection(name, material[, ...])

This method creates a GasketSection object.

GeneralStiffnessSection(name, stiffnessMatrix)

This method creates a GeneralStiffnessSection object.

HomogeneousShellSection(name, material[, ...])

This method creates a HomogeneousShellSection object.

HomogeneousSolidSection(name, material[, ...])

This method creates a HomogeneousSolidSection object.

MembraneSection(name, material[, thickness, ...])

This method creates a MembraneSection object.

MPCSection(name, mpcType[, userMode, userType])

This method creates a MPCSection object.

PEGSection(name, material[, thickness, ...])

This method creates a PEGSection object.

SurfaceSection(name[, useDensity, density])

This method creates a SurfaceSection object.

TrussSection(name, material[, area])

This method creates a TrussSection object.
Inherited from OdbBase

__init__(name[, analysisTitle, description, ...])

This method creates a new Odb object.

close()

This method closes an output database.

getFrame(frameValue[, match])

This method returns the frame at the specified time, frequency, or mode.

save()

This method saves output to an output database (.odb ) file.

update()

This method is used to update an Odb object in memory while an Abaqus analysis writes data to the associated output database.
AcousticInfiniteSection(name, material, thickness=1, order=10)[source]#

This method creates an AcousticInfiniteSection object.

Note

This function can be accessed by:

mdb.models[name].AcousticInfiniteSection
session.odbs[name].AcousticInfiniteSection

Note

Check AcousticInfiniteSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • material (str) – A String specifying the name of the material.

  • thickness (float, default: 1) – A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

  • order (int, default: 10) – An Int specifying the number of ninth-order polynomials that will be used to resolve the variation of the acoustic field in the infinite direction. Possible values are 0 << order ≤ 10. The default value is 10.

Returns:

An AcousticInfiniteSection object.

Return type:

AcousticInfiniteSection

Raises:

  • InvalidNameError –

  • RangeError –

AcousticInterfaceSection(name, thickness=1)[source]#

This method creates an AcousticInterfaceSection object.

Note

This function can be accessed by:

mdb.models[name].AcousticInterfaceSection
session.odbs[name].AcousticInterfaceSection

Note

Check AcousticInterfaceSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • thickness (float, default: 1) – A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

Returns:

An AcousticInterfaceSection object.

Return type:

AcousticInterfaceSection

Raises:

  • InvalidNameError –

  • RangeError –

BeamSection(name, integration, profile, poissonRatio=0, thermalExpansion=OFF, temperatureDependency=OFF, dependencies=0, density=None, referenceTemperature=None, temperatureVar=abaqusConstants.LINEAR, alphaDamping=0, betaDamping=0, compositeDamping=0, useFluidInertia=OFF, submerged=abaqusConstants.FULLY, fluidMassDensity=None, crossSectionRadius=None, lateralMassCoef=1, axialMassCoef=0, massOffsetX=0, massOffsetY=0, beamShape=abaqusConstants.CONSTANT, material='', table=(), outputPts=(), centroid=(), shearCenter=(), profileEnd='')[source]#

This method creates a BeamSection object.

Note

This function can be accessed by:

mdb.models[name].BeamSection
session.odbs[name].BeamSection

Note

Check BeamSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • integration (SymbolicConstant) – A SymbolicConstant specifying the integration method for the section. Possible values are BEFORE_ANALYSIS and DURING_ANALYSIS.

  • profile (str) – A String specifying the name of the profile. This argument represents the start profile in case of beamShape = TAPERED.

  • poissonRatio (float, default: 0) – A Float specifying the Poisson’s ratio of the section. The default value is 0.0.

  • thermalExpansion (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether to use thermal expansion data. The default value is OFF.

  • temperatureDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the data depend on temperature. The default value is OFF.

  • dependencies (int, default: 0) – An Int specifying the number of field variable dependencies. The default value is 0.

  • density (Optional[float], default: None) – None or a Float specifying the density of the section. The default value is None.

  • referenceTemperature (Optional[float], default: None) – None or a Float specifying the reference temperature of the section. The default value is None.

  • temperatureVar (SymbolicConstant, default: LINEAR) – A SymbolicConstant specifying the temperature variation for the section. Possible values are LINEAR and INTERPOLATED. The default value is LINEAR.

  • alphaDamping (float, default: 0) – A Float specifying the αRαR factor to create mass proportional damping in direct-integration dynamics. The default value is 0.0.

  • betaDamping (float, default: 0) – A Float specifying the βRβR factor to create stiffness proportional damping in direct-integration dynamics. The default value is 0.0.

  • compositeDamping (float, default: 0) – A Float specifying the fraction of critical damping to be used in calculating composite damping factors for the modes (for use in modal dynamics). The default value is 0.0.

  • useFluidInertia (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether added mass effects will be simulated. The default value is OFF.

  • submerged (SymbolicConstant, default: FULLY) – A SymbolicConstant specifying whether the section is either full submerged or half submerged. This argument applies only when useFluidInertia = True. Possible values are FULLY and HALF. The default value is FULLY.

  • fluidMassDensity (Optional[float], default: None) – None or a Float specifying the mass density of the fluid. This argument applies only when useFluidInertia = True and must be specified in that case. The default value is None.

  • crossSectionRadius (Optional[float], default: None) – None or a Float specifying the radius of the cylindrical cross-section. This argument applies only when useFluidInertia = True and must be specified in that case. The default value is None.

  • lateralMassCoef (float, default: 1) – A Float specifying the added mass coefficient, CACA, for lateral motions of the beam. This argument applies only when*useFluidInertia* = True. The default value is 1.0.

  • axialMassCoef (float, default: 0) – A Float specifying the added mass coefficient, C(A−E)C(A-E), for motions along the axis of the beam. This argument affects only the term added to the free end(s) of the beam, and applies only when useFluidInertia = True. The default value is 0.0.

  • massOffsetX (float, default: 0) – A Float specifying the local 1-coordinate of the center of the cylindrical cross-section with respect to the beam cross-section. This argument applies only when useFluidInertia = True. The default value is 0.0.

  • massOffsetY (float, default: 0) – A Float specifying the local 2-coordinate of the center of the cylindrical cross-section with respect to the beam cross-section. This argument applies only when useFluidInertia = True. The default value is 0.0.

  • beamShape (SymbolicConstant, default: CONSTANT) – A SymbolicConstant specifying the change in cross-section of the beam along length. Possible values are CONSTANT and TAPERED. The default value is CONSTANT. This parameter is available for manipulating the model database but not for the ODB API.

  • material (str, default: '') – A String specifying the name of the material. The default value is an empty string. The material is required when integration is “DURING_ANALYSIS”.

  • table (tuple, default: ()) – A sequence of sequences of Floats specifying the items described below. The default value is an empty sequence.

  • outputPts (tuple, default: ()) – A sequence of pairs of Floats specifying the positions at which output is requested. The default value is an empty sequence.

  • centroid (Tuple[float, ...], default: ()) – A pair of Floats specifying the X - Y coordinates of the centroid. The default value is (0.0, 0.0).

  • shearCenter (Tuple[float, ...], default: ()) – A pair of Floats specifying the X - Y coordinates of the shear center. The default value is (0.0, 0.0).

  • profileEnd (str, default: '') – A String specifying the name of the end profile. The type of the end profile must be same as that of the start profile. This argument is valid only when beamShape = TAPERED. The default value is an empty string. This parameter is available for manipulating the model database but not for the ODB API.

Returns:

A BeamSection object.

Return type:

BeamSection

CohesiveSection(name, response, material, initialThicknessType=abaqusConstants.SOLVER_DEFAULT, initialThickness=1, outOfPlaneThickness=None)[source]#

This method creates a CohesiveSection object.

Note

This function can be accessed by:

mdb.models[name].CohesiveSection
session.odbs[name].CohesiveSection

Note

Check CohesiveSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • response (SymbolicConstant) – A SymbolicConstant specifying the geometric assumption that defines the constitutive behavior of the cohesive elements. Possible values are TRACTION_SEPARATION, CONTINUUM, and GASKET.

  • material (str) – A String specifying the name of the material.

  • initialThicknessType (SymbolicConstant, default: SOLVER_DEFAULT) – A SymbolicConstant specifying the method used to compute the initial thickness. Possible values are:SOLVER_DEFAULT, specifying that Abaqus will use the analysis product defaultGEOMETRY, specifying that Abaqus will compute the thickness from the nodal coordinates of the elements.SPECIFY, specifying that Abaqus will use the value given for initialThickness The default value is SOLVER_DEFAULT.

  • initialThickness (float, default: 1) – A Float specifying the initial thickness for the section. The initialThickness argument applies only when initialThicknessType = SPECIFY. The default value is 1.0.

  • outOfPlaneThickness (Optional[float], default: None) – None or a Float specifying the out-of-plane thickness for the section. The default value is None.

Returns:

A CohesiveSection object.

Return type:

CohesiveSection

Raises:

RangeError –

CompositeShellSection(name, layup, symmetric=OFF, thicknessType=abaqusConstants.UNIFORM, preIntegrate=OFF, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, integrationRule=abaqusConstants.SIMPSON, temperature=abaqusConstants.GRADIENT, idealization=abaqusConstants.NO_IDEALIZATION, nTemp=None, thicknessModulus=None, useDensity=OFF, density=0, layupName='', thicknessField='', nodalThicknessField='')[source]#

This method creates a CompositeShellSection object.

Note

This function can be accessed by:

mdb.models[name].parts[name].compositeLayups[i].CompositeShellSection
mdb.models[name].CompositeShellSection
session.odbs[name].CompositeShellSection

Note

Check CompositeShellSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • layup (List[SectionLayer]) – A SectionLayerArray object specifying the shell cross-section.

  • symmetric (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.

  • thicknessType (SymbolicConstant, default: UNIFORM) – A SymbolicConstant specifying the distribution used for defining the thickness of the elements. Possible values are UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, and NODAL_DISCRETE_FIELD. The default value is UNIFORM.

  • preIntegrate (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the shell section properties are specified by the user prior to the analysis (ON) or integrated during the analysis (OFF). The default value is OFF.

  • poissonDefinition (SymbolicConstant, default: DEFAULT) – A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

  • poisson (float, default: 0) – A Float specifying the Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

  • integrationRule (SymbolicConstant, default: SIMPSON) – A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.

  • temperature (SymbolicConstant, default: GRADIENT) – A SymbolicConstant specifying the mode used for temperature and field variable input across the section thickness. Possible values are GRADIENT and POINTWISE. The default value is GRADIENT.

  • idealization (SymbolicConstant, default: NO_IDEALIZATION) – A SymbolicConstant specifying the mechanical idealization used for the section calculations. This member is only applicable when preIntegrate is set to ON. Possible values are NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, and BENDING. The default value is NO_IDEALIZATION.

  • nTemp (Optional[int], default: None) – None or an Int specifying the number of temperature points to be input. This argument is valid only when temperature = POINTWISE. The default value is None.

  • thicknessModulus (Optional[float], default: None) – None or a Float specifying the effective thickness modulus. This argument is relevant only for continuum shells and must be used in conjunction with the argument poisson. The default value is None.

  • useDensity (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not to use the value of density. The default value is OFF.

  • density (float, default: 0) – A Float specifying the value of density to apply to this section. The default value is 0.0.

  • layupName (str, default: '') – A String specifying the layup name for this section. The default value is an empty string.

  • thicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements. The thicknessField argument applies only when thicknessType = ANALYTICAL_FIELD or thicknessType = DISCRETE_FIELD. The default value is an empty string.

  • nodalThicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements at each node. The nodalThicknessField argument applies only when thicknessType = NODAL_ANALYTICAL_FIELD or thicknessType = NODAL_DISCRETE_FIELD. The default value is an empty string.

Returns:

A CompositeShellSection object.

Return type:

CompositeShellSection

CompositeSolidSection(name, layup, symmetric=OFF, layupName='')[source]#

This method creates a CompositeSolidSection object.

Note

This function can be accessed by:

mdb.models[name].CompositeSolidSection
session.odbs[name].CompositeSolidSection

Note

Check CompositeSolidSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • layup (List[SectionLayer]) – A SectionLayerArray object specifying the solid cross-section.

  • symmetric (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.

  • layupName (str, default: '') – A String specifying the layup name for this section. The default value is an empty string.

Returns:

A CompositeSolidSection object.

Return type:

CompositeSolidSection

ConnectorSection(name, assembledType=abaqusConstants.NONE, rotationalType=abaqusConstants.NONE, translationalType=abaqusConstants.NONE, integration=abaqusConstants.UNSPECIFIED, u1ReferenceLength=None, u2ReferenceLength=None, u3ReferenceLength=None, ur1ReferenceAngle=None, ur2ReferenceAngle=None, ur3ReferenceAngle=None, massPerLength=None, contactAngle=None, materialFlowFactor=1, regularize=ON, defaultTolerance=ON, regularization=0, extrapolation=abaqusConstants.CONSTANT, behaviorOptions=None)[source]#

This method creates a ConnectorSection object.

Note

This function can be accessed by:

mdb.models[name].ConnectorSection
session.odbs[name].ConnectorSection

Note

Check ConnectorSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • assembledType (SymbolicConstant, default: NONE) – A SymbolicConstant specifying the assembled connection type. Possible values are:NONEBEAMBUSHINGCVJOINTCYLINDRICALHINGEPLANARRETRACTORSLIPRINGTRANSLATORUJOINTWELDThe default value is NONE.You cannot include the assembledType argument if translationalType or rotationalType are given a value other than NONE. At least one of the arguments assembledType, translationalType, or rotationalType must be given a value other than NONE.

  • rotationalType (SymbolicConstant, default: NONE) – A SymbolicConstant specifying the basic rotational connection type. Possible values are:NONEALIGNCARDANCONSTANT_VELOCITYEULERFLEXION_TORSIONFLOW_CONVERTERPROJECTION_FLEXION_TORSIONREVOLUTEROTATIONROTATION_ACCELEROMETERUNIVERSALThe default value is NONE.You cannot include the rotationalType argument if assembledType is given a value other than NONE. At least one of the arguments assembledType, translationalType, or rotationalType must be given an value other than NONE.

  • translationalType (SymbolicConstant, default: NONE) – A SymbolicConstant specifying the basic translational connection type. Possible values are:NONEACCELEROMETERAXIALCARTESIANJOINLINKPROJECTION_CARTESIANRADIAL_THRUSTSLIDE_PLANESLOTThe default value is NONE.You cannot include the translationalType argument if assembledType is given a value other than NONE. At least one of the arguments assembledType, translationalType, or rotationalType must be given an value other than NONE.

  • integration (SymbolicConstant, default: UNSPECIFIED) – A SymbolicConstant specifying the time integration scheme to use for analysis. This argument is applicable only to an Abaqus/Explicit analysis. Possible values are UNSPECIFIED, IMPLICIT, and EXPLICIT. The default value is UNSPECIFIED.

  • u1ReferenceLength (Optional[float], default: None) – None or a Float specifying the reference length associated with constitutive response for the first component of relative motion. The default value is None.

  • u2ReferenceLength (Optional[float], default: None) – None or a Float specifying the reference length associated with constitutive response for the second component of relative motion. The default value is None.

  • u3ReferenceLength (Optional[float], default: None) – None or a Float specifying the reference length associated with constitutive response for the third component of relative motion. The default value is None.

  • ur1ReferenceAngle (Optional[float], default: None) – None or a Float specifying the reference angle in degrees associated with constitutive response for the fourth component of relative motion. The default value is None.

  • ur2ReferenceAngle (Optional[float], default: None) – None or a Float specifying the reference angle in degrees associated with constitutive response for the fifth component of relative motion. The default value is None.

  • ur3ReferenceAngle (Optional[float], default: None) – None or a Float specifying the reference angle in degrees associated with constitutive response for the sixth component of relative motion. The default value is None.

  • massPerLength (Optional[float], default: None) – None or a Float specifying the mass per unit reference length of belt material. This argument is applicable only when assembledType = SLIPRING, and must be specified in that case. The default value is None.

  • contactAngle (Optional[float], default: None) – None or a Float specifying the contact angle made by the belt wrapping around node b. This argument is applicable only to an Abaqus/Explicit analysis, and only when assembledType = SLIPRING. The default value is None.

  • materialFlowFactor (float, default: 1) – A Float specifying the scaling factor for material flow at node b. This argument is applicable only when assembledType = RETRACTOR or rotationalType = FLOW_CONVERTER. The default value is 1.0.

  • regularize (Union[AbaqusBoolean, bool], default: ON) – A Boolean specifying whether or not all tabular data associated with the behaviorOptions will be regularized. This argument is applicable only for an Abaqus/Explicit analysis. The default value is ON.

  • defaultTolerance (Union[AbaqusBoolean, bool], default: ON) – A Boolean specifying whether or not the default regularization tolerance will be used for all tabular data associated with the behaviorOptions. This argument is applicable only for an Abaqus/Explicit analysis and only if regularize = ON. The default value is ON.

  • regularization (float, default: 0) – A Float specifying the regularization increment to be used for all tabular data associated with the behaviorOptions. This argument is applicable only for an Abaqus/Explicit analysis and only if regularize = ON and defaultTolerance = OFF. The default value is 0.03.

  • extrapolation (SymbolicConstant, default: CONSTANT) – A SymbolicConstant specifying the extrapolation technique to be used for all tabular data associated with the behaviorOptions. Possible values are CONSTANT and LINEAR. The default value is CONSTANT.

  • behaviorOptions (Optional[List[ConnectorBehaviorOption]], default: None) – A ConnectorBehaviorOptionArray object.

Returns:

A ConnectorSection object.

Return type:

ConnectorSection

Raises:

  • InvalidNameError –

  • RangeError –

EulerianSection(name, data)[source]#

This method creates a EulerianSection object.

Note

This function can be accessed by:

mdb.models[name].EulerianSection
session.odbs[name].EulerianSection

Note

Check EulerianSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • data (str) – A String-to-String Dictionary specifying a dictionary mapping Material instance names to Material names. Internally the specified mapping gets sorted on Material instance name.

Returns:

An EulerianSection object.

Return type:

EulerianSection

GasketSection(name, material, crossSection=1, initialGap=0, initialThickness=abaqusConstants.DEFAULT, initialVoid=0, stabilizationStiffness=abaqusConstants.DEFAULT)[source]#

This method creates a GasketSection object.

Note

This function can be accessed by:

mdb.models[name].GasketSection
session.odbs[name].GasketSection

Note

Check GasketSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • material (str) – A String specifying the name of the material of which the gasket is made or material that defines gasket behavior.

  • crossSection (float, default: 1) – A Float specifying the cross-sectional area, width, or out-of-plane thickness, if applicable, depending on the gasket element type. The default value is 1.0.

  • initialGap (float, default: 0) – A Float specifying the initial gap. The default value is 0.0.

  • initialThickness (Union[SymbolicConstant, float], default: DEFAULT) – The SymbolicConstant DEFAULT or a Float specifying the initial gasket thickness. If DEFAULT is specified, the initial thickness is determined using nodal coordinates. The default value is DEFAULT.

  • initialVoid (float, default: 0) – A Float specifying the initial void. The default value is 0.0.

  • stabilizationStiffness (Union[SymbolicConstant, float], default: DEFAULT) – The SymbolicConstant DEFAULT or a Float specifying the default stabilization stiffness used in all but link elements to stabilize gasket elements that are not supported at all nodes, such as those that extend outside neighboring components. If DEFAULT is specified, a value is used equal to 10-9 times the initial compressive stiffness in the thickness direction. The default value is DEFAULT.

Returns:

A GasketSection object. and ValueError.

Return type:

GasketSection

GeneralStiffnessSection(name, stiffnessMatrix, referenceTemperature=None, applyThermalStress=OFF, temperatureDependency=OFF, dependencies=0, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, useDensity=OFF, density=0, thermalStresses=(), scalingData=())[source]#

This method creates a GeneralStiffnessSection object.

Note

This function can be accessed by:

mdb.models[name].GeneralStiffnessSection
session.odbs[name].GeneralStiffnessSection

Note

Check GeneralStiffnessSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • stiffnessMatrix (tuple) – A sequence of Floats specifying the stiffness matrix for the section in the order D11, D12, D22, D13, D23, D33, …., D66. Twenty-one entries must be given.

  • referenceTemperature (Optional[float], default: None) – None or a Float specifying the reference temperature for thermal expansion. The default value is None.

  • applyThermalStress (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not the section stiffness varies with thermal stresses. The default value is OFF.

  • temperatureDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the data depend on temperature. The default value is OFF.

  • dependencies (int, default: 0) – An Int specifying the number of field variable dependencies. The default value is 0.

  • poissonDefinition (SymbolicConstant, default: DEFAULT) – A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

  • poisson (float, default: 0) – A Float specifying the Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

  • useDensity (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not to use the value of density. The default value is OFF.

  • density (float, default: 0) – A Float specifying the value of density to apply to this section. The default value is 0.0.

  • thermalStresses (tuple, default: ()) – A sequence of Floats specifying the generalized stress values caused by a unit temperature rise. Six entries must be given if the value of applyThermalStress is set to True. The default value is (“”).

  • scalingData (tuple, default: ()) – A sequence of sequences of Floats specifying the scaling factors for given temperatures and/or field data. Each row should contain (Y, alpha, T, F1,…,Fn). The default value is an empty sequence.

Returns:

A GeneralStiffnessSection object.

Return type:

GeneralStiffnessSection

HomogeneousShellSection(name, material, thickness=0, numIntPts=5, thicknessType=abaqusConstants.UNIFORM, preIntegrate=OFF, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, integrationRule=abaqusConstants.SIMPSON, temperature=abaqusConstants.GRADIENT, idealization=abaqusConstants.NO_IDEALIZATION, nTemp=None, thicknessModulus=None, useDensity=OFF, density=0, thicknessField='', nodalThicknessField='')[source]#

This method creates a HomogeneousShellSection object.

Note

This function can be accessed by:

mdb.models[name].parts[name].compositeLayups[i].HomogeneousShellSection
mdb.models[name].HomogeneousShellSection
session.odbs[name].HomogeneousShellSection

Note

Check HomogeneousShellSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • material (str) – A String specifying the name of the section material.

  • thickness (float, default: 0) – A Float specifying the thickness of the section. The thickness argument applies only when thicknessType = UNIFORM. The default value is 0.0.

  • numIntPts (int, default: 5) – An Int specifying the number of integration points to be used through the section. Possible values are numIntPts >> 0. The default value is 5.To use the default settings of the analysis products, set numIntPts to 5 if integrationRule = SIMPSON or set numIntPts to 7 if integrationRule = GAUSS.

  • thicknessType (SymbolicConstant, default: UNIFORM) – A SymbolicConstant specifying the distribution used for defining the thickness of the elements. Possible values are UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, and NODAL_DISCRETE_FIELD. The default value is UNIFORM.

  • preIntegrate (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the shell section properties are specified by the user prior to the analysis (ON) or integrated during the analysis (OFF). The default value is OFF.

  • poissonDefinition (SymbolicConstant, default: DEFAULT) – A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

  • poisson (float, default: 0) – A Float specifying the Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

  • integrationRule (SymbolicConstant, default: SIMPSON) – A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.

  • temperature (SymbolicConstant, default: GRADIENT) – A SymbolicConstant specifying the mode used for temperature and field variable input across the section thickness. Possible values are GRADIENT and POINTWISE. The default value is GRADIENT.

  • idealization (SymbolicConstant, default: NO_IDEALIZATION) – A SymbolicConstant specifying the mechanical idealization used for the section calculations. This member is only applicable when preIntegrate is set to ON. Possible values are NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, and BENDING. The default value is NO_IDEALIZATION.

  • nTemp (Optional[int], default: None) – None or an Int specifying the number of temperature points to be input. This argument is valid only when temperature = POINTWISE. The default value is None.

  • thicknessModulus (Optional[float], default: None) – None or a Float specifying the effective thickness modulus. This argument is relevant only for continuum shells and must be used in conjunction with the argument poisson. The default value is None.

  • useDensity (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not to use the value of density. The default value is OFF.

  • density (float, default: 0) – A Float specifying the value of density to apply to this section. The default value is 0.0.

  • thicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements. The thicknessField argument applies only when thicknessType = ANALYTICAL_FIELD or thicknessType = DISCRETE_FIELD. The default value is an empty string.

  • nodalThicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements at each node. The nodalThicknessField argument applies only when thicknessType = NODAL_ANALYTICAL_FIELD or thicknessType = NODAL_DISCRETE_FIELD. The default value is an empty string.

Returns:

A HomogeneousShellSection object.

Return type:

HomogeneousShellSection

HomogeneousSolidSection(name, material, thickness=1)[source]#

This method creates a HomogeneousSolidSection object.

Note

This function can be accessed by:

mdb.models[name].HomogeneousSolidSection
session.odbs[name].HomogeneousSolidSection

Note

Check HomogeneousSolidSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • material (str) – A String specifying the name of the material.

  • thickness (float, default: 1) –

    A Float specifying the thickness of the section. Possible values are None or greater than zero. The default value is 1.0.

    Changed in version 2018: The default value is now 1.0 instead of None.

Returns:

A HomogeneousSolidSection object.

Return type:

HomogeneousSolidSection

Raises:

  • InvalidNameError –

  • RangeError –

MPCSection(name, mpcType, userMode=abaqusConstants.DOF_MODE, userType=0)[source]#

This method creates a MPCSection object.

Note

This function can be accessed by:

mdb.models[name].MPCSection
session.odbs[name].MPCSection

Note

Check MPCSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • mpcType (SymbolicConstant) – A SymbolicConstant specifying the MPC type of the section. Possible values are BEAM_MPC, ELBOW_MPC, PIN_MPC, LINK_MPC, TIE_MPC, and USER_DEFINED.

  • userMode (SymbolicConstant, default: DOF_MODE) – A SymbolicConstant specifying the mode of the MPC when it is user-defined. Possible values are DOF_MODE and NODE_MODE. The default value is DOF_MODE.The userMode argument applies only when mpcType = USER_DEFINED.

  • userType (int, default: 0) – An Int specifying to differentiate between different constraint types in a user-defined MPCSection. The default value is 0.The userType argument applies only when mpcType = USER_DEFINED.

Returns:

A MPCSection object.

Return type:

MPCSection

Raises:

RangeError –

MembraneSection(name, material, thickness=1, thicknessType=abaqusConstants.UNIFORM, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, thicknessField='')[source]#

This method creates a MembraneSection object.

Note

This function can be accessed by:

mdb.models[name].MembraneSection
session.odbs[name].MembraneSection

Note

Check MembraneSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • material (str) – A String specifying the name of the material.

  • thickness (float, default: 1) – A Float specifying the thickness for the section. Possible values are thickness >> 0.0. The default value is 1.0.

  • thicknessType (SymbolicConstant, default: UNIFORM) – A SymbolicConstant specifying the distribution used for defining the thickness of the elements. Possible values are UNIFORM, ANALYTICAL_FIELD, and DISCRETE_FIELD. The default value is UNIFORM.

  • poissonDefinition (SymbolicConstant, default: DEFAULT) – A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

  • poisson (float, default: 0) – A Float specifying the section Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

  • thicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements. The thicknessField argument applies only when thicknessType = ANALYTICAL_FIELD or thicknessType = DISCRETE_FIELD. The default value is an empty string.

Returns:

A MembraneSection object.

Return type:

MembraneSection

Raises:

RangeError –

PEGSection(name, material, thickness=1, wedgeAngle1=0, wedgeAngle2=0)[source]#

This method creates a PEGSection object.

Note

This function can be accessed by:

mdb.models[name].PEGSection
session.odbs[name].PEGSection

Note

Check PEGSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • material (str) – A String specifying the name of the material.

  • thickness (float, default: 1) – A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

  • wedgeAngle1 (float, default: 0) – A Float specifying the value of the x component of the angle between the bounding planes, ΔϕxΔ⁢ϕx. The default value is 0.0.

  • wedgeAngle2 (float, default: 0) – A Float specifying the value of the y component of the angle between the bounding planes, ΔϕyΔ⁢ϕy. The default value is 0.0.

Returns:

A PEGSection object.

Return type:

PEGSection

Raises:

  • InvalidNameError –

  • RangeError –

SurfaceSection(name, useDensity=OFF, density=0)[source]#

This method creates a SurfaceSection object.

Note

This function can be accessed by:

mdb.models[name].SurfaceSection
session.odbs[name].SurfaceSection

Note

Check SurfaceSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • useDensity (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not to use the value of density. The default value is OFF.

  • density (float, default: 0) – A Float specifying the value of density to apply to this section. The default value is 0.0.

Returns:

A SurfaceSection object.

Return type:

SurfaceSection

Raises:

RangeError –

TrussSection(name, material, area=1)[source]#

This method creates a TrussSection object.

Note

This function can be accessed by:

mdb.models[name].TrussSection
session.odbs[name].TrussSection

Note

Check TrussSection on help.3ds.com/0.1..

Parameters:

  • name (str) – A String specifying the repository key.

  • material (str) – A String specifying the name of the material.

  • area (float, default: 1) – A Float specifying the cross-sectional area for the section. Possible values are area >> 0. The default value is 1.0.

Returns:

A TrussSection object.

Return type:

TrussSection

Raises:

RangeError –

Object features#

Section#

class Section[source]#

Public Data Attributes:

Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
ConnectorDamage(coupling=abaqusConstants.UNCOUPLED, criterion=abaqusConstants.FORCE, initiationTemperature=OFF, initiationPotentialOperator=abaqusConstants.SUM, initiationPotentialExponent=2, initiationDependencies=0, evolution=ON, evolutionType=abaqusConstants.MOTION_TYPE, softening=abaqusConstants.LINEAR, useAffected=OFF, degradation=abaqusConstants.MAXIMUM, evolutionTemperature=OFF, evolutionDependencies=0, evolutionPotentialOperator=abaqusConstants.SUM, evolutionPotentialExponent=2, initiationPotentials=None, evolutionPotentials=None, initiationTable=(), evolutionTable=(), affectedComponents=(), components=())[source]#

This method creates a connector damage behavior option for a ConnectorSection object.

Note

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorDamage
import odbConnectorBehavior
odbConnectorBehavior.ConnectorDamage

Note

Check ConnectorDamage on help.3ds.com/0.1..

Parameters:

  • coupling (SymbolicConstant, default: UNCOUPLED) – A SymbolicConstant specifying whether or not the behavior is coupled. Possible values are UNCOUPLED and COUPLED. The default value is UNCOUPLED.

  • criterion (SymbolicConstant, default: FORCE) – A SymbolicConstant specifying the damage initiation criterion to be used. Possible values are FORCE, MOTION, and PLASTIC_MOTION. The default value is FORCE.

  • initiationTemperature (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the initiation data depend on temperature. The default value is OFF.

  • initiationPotentialOperator (SymbolicConstant, default: SUM) – A SymbolicConstant specifying the contribution operator for the initiation potential contributions. Possible values are SUM and MAXIMUM. The default value is SUM.This argument is only if coupling = COUPLED and if criterion = FORCE or MOTION.

  • initiationPotentialExponent (float, default: 2) – A Float specifying the number equal to the inverse of the overall exponent in the initiation potential definition. The default value is 2.0.This argument is applicable only if coupling = COUPLED, when initiationPotentialOperator = SUM, and when criterion = FORCE or MOTION.

  • initiationDependencies (int, default: 0) – An Int specifying the number of field variable dependencies for the initiation data. The default value is 0.

  • evolution (Union[AbaqusBoolean, bool], default: ON) – A Boolean specifying whether damage evolution data will be used. The default value is ON.

  • evolutionType (SymbolicConstant, default: MOTION_TYPE) – A SymbolicConstant specifying the type of damage evolution to be specified. Possible values are MOTION_TYPE and ENERGY_TYPE. The default value is MOTION_TYPE.This argument is applicable only if evolution = ON.

  • softening (SymbolicConstant, default: LINEAR) – A SymbolicConstant specifying the damage evolution law to be specified. Possible values are LINEAR, EXPONENTIAL, and TABULAR. The default value is LINEAR.This argument is applicable only if evolution = ON and when evolutionType = MOTION_TYPE.

  • useAffected (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not affectedComponents will be specified. If useAffected = OFF, then only the components of relative motion specified by components will undergo damage. The default value is OFF.This argument is applicable only if evolution = ON.

  • degradation (SymbolicConstant, default: MAXIMUM) – A SymbolicConstant specifying the contribution of each damage mechanism when more than one damage mechanism is defined. Possible values are MAXIMUM and MULTIPLICATIVE. The default value is MAXIMUM.This argument is applicable if evolution = ON.

  • evolutionTemperature (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the evolution data depend on temperature. The default value is OFF.This argument is applicable only if evolution = ON.

  • evolutionDependencies (int, default: 0) – An Int specifying the number of field variable dependencies for the evolution data. The default value is 0.This argument is applicable only if evolution = ON.

  • evolutionPotentialOperator (SymbolicConstant, default: SUM) – A SymbolicConstant specifying the contribution operator for the evolution potential contributions. Possible values are SUM and MAXIMUM. The default value is SUM.This argument is applicable only if coupling = COUPLED, when evolution = ON, when evolutionType = MOTION_TYPE, and when criterion = FORCE or MOTION.

  • evolutionPotentialExponent (float, default: 2) – A Float specifying the number equal to the inverse of the overall exponent in the evolution potential definition. The default value is 2.0.This argument is applicable only if coupling = COUPLED, when evolution = ON, when evolutionPotentialOperator = SUM, when evolutionType = MOTION, and when criterion = FORCE or MOTION.

  • initiationPotentials (Optional[List[ConnectorPotential]], default: None) – A ConnectorPotentialArray object specifying one ConnectorPotential object for each initiation potential contribution. This member can be specified only if coupling = COUPLED and if criterion = FORCE or MOTION.

  • evolutionPotentials (Optional[List[ConnectorPotential]], default: None) – A ConnectorPotentialArray object specifying one ConnectorPotential object for each evolution potential contribution). This member can be specified only if coupling = COUPLED, if evolution = ON, if evolutionType = MOTION, and if criterion = FORCE or MOTION.

  • initiationTable (tuple, default: ()) – A sequence of sequences of Floats specifying the initiation properties. The default value is an empty sequence.Items in the initiationTable data are described below.

  • evolutionTable (tuple, default: ()) – A sequence of sequences of Floats specifying the evolution properties. The default value is an empty sequence.Items in the evolutionTable data are described below. This argument is only applicable if evolution = ON.

  • affectedComponents (tuple, default: ()) – A sequence of Ints specifying the components of relative motion that will be damaged. Possible values are 1 ≤ components ≤ 6. Only available components can be specified. This argument is applicable only if evolution = ON and useAffected = ON. The default value is an empty sequence.

  • components (tuple, default: ()) – A sequence of Ints specifying the components of relative motion for which the behavior is defined. Possible values are 1 ≤ components ≤ 6. Only available components can be specified. This argument can be specified only if coupling = UNCOUPLED. The default value is an empty sequence.

Returns:

A ConnectorDamage object.

Return type:

ConnectorDamage

Raises:

ValueError –

ConnectorDamping(type=abaqusConstants.VISCOUS, behavior=abaqusConstants.LINEAR, coupling=abaqusConstants.UNCOUPLED, dependencies=0, temperatureDependency=OFF, frequencyDependency=OFF, table=(), independentComponents=(), components=())[source]#

This method creates a connector damping behavior option for a ConnectorSection object.

Note

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorDamping
import odbConnectorBehavior
odbConnectorBehavior.ConnectorDamping

Note

Check ConnectorDamping on help.3ds.com/0.1..

Parameters:

  • type (SymbolicConstant, default: VISCOUS) –

    A SymbolicConstant specifying if the damping type is viscous or structural. Possible values are VISCOUS and STRUCTURAL. The default value is VISCOUS.

    New in version 2022: The type argument was added.

  • behavior (SymbolicConstant, default: LINEAR) – A SymbolicConstant specifying if the damping behavior is linear or nonlinear. Possible values are LINEAR and NONLINEAR. The default value is LINEAR.

  • coupling (SymbolicConstant, default: UNCOUPLED) – A SymbolicConstant specifying whether the damping behavior is coupled between the connector’s components of relative motion. If behavior = LINEAR, then possible values are UNCOUPLED and COUPLED. If behavior = NONLINEAR, then possible values are UNCOUPLED, COUPLED_POSITION, and COUPLED_MOTION. Possible values are UNCOUPLED, COUPLED, COUPLED_POSITION, and COUPLED_MOTION. The default value is UNCOUPLED.

  • dependencies (int, default: 0) – An Int specifying the number of field variable dependencies. The default value is 0.

  • temperatureDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the behavior data depend on temperature. The default value is OFF.

  • frequencyDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the behavior data depend on frequency. This value is applicable only if behavior = LINEAR and coupling = UNCOUPLED. The default value is OFF.

  • table (tuple, default: ()) – A sequence of sequences of Floats specifying damping properties. Items in the table data are described below. The default value is an empty sequence.

  • independentComponents (tuple, default: ()) – A sequence of Ints specifying the list of independent components that are included in the definition of the connector damping data. This argument is applicable only if behavior = NONLINEAR and coupling = COUPLED_POSITION or COUPLED_MOTION. When this argument is applicable, at least one value must be specified. Only available components can be specified. The default value is an empty sequence.

  • components (tuple, default: ()) – A sequence of Ints specifying the components of relative motion for which the behavior is defined. Possible values are 1 ≤ components ≤ 6. Only available components can be specified. The default value is an empty sequence.

Returns:

A ConnectorDamping object.

Return type:

ConnectorDamping

Raises:

ValueError –

ConnectorElasticity(behavior=abaqusConstants.LINEAR, coupling=abaqusConstants.UNCOUPLED, dependencies=0, temperatureDependency=OFF, frequencyDependency=OFF, table=(), independentComponents=(), components=())[source]#

This method creates a connector elasticity behavior option for a ConnectorSection object.

Note

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorElasticity
import odbConnectorBehavior
odbConnectorBehavior.ConnectorElasticity

Note

Check ConnectorElasticity on help.3ds.com/0.1..

Parameters:

  • behavior (SymbolicConstant, default: LINEAR) – A SymbolicConstant specifying whether the elastic behavior is linear, nonlinear, or rigid. Possible values are LINEAR, NONLINEAR, and RIGID. The default value is LINEAR.

  • coupling (SymbolicConstant, default: UNCOUPLED) – A SymbolicConstant specifying whether the elastic behavior is coupled between the connector’s components of relative motion. If behavior = LINEAR, then possible values are UNCOUPLED and COUPLED. If behavior = NONLINEAR, then possible values are UNCOUPLED, COUPLED_POSITION, and COUPLED_MOTION. Possible values are UNCOUPLED, COUPLED, COUPLED_POSITION, and COUPLED_MOTION. The default value is UNCOUPLED.This argument is not applicable if behavior = RIGID.

  • dependencies (int, default: 0) – An Int specifying the number of field variable dependencies. The default value is 0.This argument is not applicable if behavior = RIGID.

  • temperatureDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the behavior data depend on temperature. The default value is OFF.This argument is not applicable if behavior = RIGID.

  • frequencyDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the behavior data depend on frequency. This value is applicable only if behavior = LINEAR and coupling = UNCOUPLED. The default value is OFF.This argument is not applicable if behavior = RIGID.

  • table (tuple, default: ()) – A sequence of sequences of Floats specifying elasticity properties. Items in the table data are described below. This argument is not applicable if behavior = RIGID. The default value is an empty sequence.

  • independentComponents (tuple, default: ()) – A sequence of Ints specifying the list of independent components that are included in the definition of the connector elasticity data. This argument is applicable only if behavior = NONLINEAR and coupling = COUPLED_POSITION or COUPLED_MOTION. If this argument is applicable, at least one value must be specified. Only available components can be specified. The default value is an empty sequence.

  • components (tuple, default: ()) – A sequence of Ints specifying the components of relative motion for which the behavior is defined. Possible values are 1 ≤ components ≤ 6. Only available components can be specified. The default value is an empty sequence.

Returns:

A ConnectorElasticity object.

Return type:

ConnectorElasticity

Raises:

ValueError –

ConnectorFailure(releaseComponent=abaqusConstants.ALL, minMotion=None, maxMotion=None, minForce=None, maxForce=None, components=())[source]#

This method creates a connector failure behavior option for a ConnectorSection object.

Note

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorFailure
import odbConnectorBehavior
odbConnectorBehavior.ConnectorFailure

Note

Check ConnectorFailure on help.3ds.com/0.1..

Parameters:

  • releaseComponent (SymbolicConstant, default: ALL) – The SymbolicConstant ALL or an Int specifying the motion components that fail. If an Int is specified, only that motion component fails when the failure criteria are satisfied. If releaseComponent = ALL, all motion components fail. The default value is ALL.

  • minMotion (Optional[float], default: None) – None or a Float specifying the lower bound for the connector’s relative position for all specified components, or no lower bound. The default value is None.

  • maxMotion (Optional[float], default: None) – None or a Float specifying the upper bound for the connector’s relative position for all specified components, or no upper bound. The default value is None.

  • minForce (Optional[float], default: None) – None or a Float specifying the lower bound of the force or moment in the directions of the specified components at which locking occurs, or no lower bound. The default value is None.

  • maxForce (Optional[float], default: None) – None or a Float specifying the upper bound of the force or moment in the directions of the specified components at which locking occurs, or no upper bound. The default value is None.

  • components (tuple, default: ()) – A sequence of Ints specifying the components of relative motion for which the behavior is defined. Possible values are 1 ≤ components ≤ 6. Only available components can be specified. The default value is an empty sequence.

Returns:

A ConnectorFailure object.

Return type:

ConnectorFailure

Raises:

ValueError –

ConnectorFriction(frictionModel=abaqusConstants.PREDEFINED, slipStyle=abaqusConstants.SPECIFY, tangentDirection=None, stickStiffness=None, componentType=abaqusConstants.NO_INDEPENDENT_COMPONENTS, slipDependency=OFF, temperatureDependency=OFF, dependencies=0, useContactForceComponent=OFF, contactForceStyle=abaqusConstants.COMPONENT_NUMBER, contactForceComponent=0, forcePotentialOperator=abaqusConstants.SUM, forcePotentialExponent=2, connectorPotentials=None, table=(), independentComponents=())[source]#

This method creates a connector friction behavior option for a ConnectorSection object. Depending upon the arguments provided, the friction behavior can be Coulomb-like or hysteretic in nature.

Note

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorFriction
import odbConnectorBehavior
odbConnectorBehavior.ConnectorFriction

Note

Check ConnectorFriction on help.3ds.com/0.1..

Parameters:

  • frictionModel (SymbolicConstant, default: PREDEFINED) – A SymbolicConstant specifying the desired frictional response model. Possible values are PREDEFINED and USER_CUSTOMIZED. The default value is PREDEFINED.

  • slipStyle (SymbolicConstant, default: SPECIFY) – A SymbolicConstant specifying the method of indicating the slip direction: either specified or computed based upon the force potential data. Possible values are SPECIFY and COMPUTE. The default value is SPECIFY.This argument is applicable only if frictionModel = USER_CUSTOMIZED.

  • tangentDirection (Optional[int], default: None) – None or an Int specifying the direction for which the frictional behavior is specified. Possible values are 1 ≤ tangentDirection ≤ 6, indicating an available component of relative motion. This argument applies only if frictionModel = USER_CUSTOMIZED and if slipStyle = SPECIFY. The default value is None.

  • stickStiffness (Optional[float], default: None) – None or a Float specifying the stick stiffness associated with the frictional behavior in the direction specified by tangentDirection. If this argument is omitted, Abaqus computes an appropriate number for the stick stiffness. The default value is None.

  • componentType (SymbolicConstant, default: NO_INDEPENDENT_COMPONENTS) – A SymbolicConstant specifying the type of the independentComponents. Possible values are POSITION, MOTION, and NO_INDEPENDENT_COMPONENTS. The default value is NO_INDEPENDENT_COMPONENTS.

  • slipDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the table data depend on accumulated slip. The default value is OFF.This argument applies only if frictionModel = USER_CUSTOMIZED.

  • temperatureDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the table data depend on temperature. The default value is OFF.This argument applies only if frictionModel = USER_CUSTOMIZED.

  • dependencies (int, default: 0) – An Int specifying the number of field variable dependencies. The default value is 0.This argument applies only if frictionModel = USER_CUSTOMIZED.

  • useContactForceComponent (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the contact force component will be defined. The default value is OFF.This argument applies only if frictionModel = USER_CUSTOMIZED.

  • contactForceStyle (SymbolicConstant, default: COMPONENT_NUMBER) – A SymbolicConstant specifying the method of indicating the contact force component direction: either specified or computed based on upon a DerivedComponent. Possible values are COMPONENT_NUMBER and DERIVED_COMPONENT. The default value is COMPONENT_NUMBER.This argument is applicable only if frictionModel = USER_CUSTOMIZED and if useContactForceComponent = ON.

  • contactForceComponent (int, default: 0) – An Int specifying the contact force component direction. This argument applies only if frictionModel = USER_CUSTOMIZED, if useContactForceComponent = ON, and if contactForceStyle = COMPONENT_NUMBER. The default value is 0.

  • forcePotentialOperator (SymbolicConstant, default: SUM) – A SymbolicConstant specifying the contribution operator for the force potential contributions. Possible values are SUM and MAXIMUM. The default value is SUM.This argument is applicable only if frictionModel = USER_CUSTOMIZED and if slipStyle = COMPUTE.

  • forcePotentialExponent (float, default: 2) – A Float specifying the number equal to the inverse of the overall exponent in the force potential definition. The default value is 2.0.This argument is applicable only if frictionModel = USER_CUSTOMIZED, if slipStyle = COMPUTE, and if forcePotentialOperator = SUM.

  • connectorPotentials (Optional[List[ConnectorPotential]], default: None) – A ConnectorPotentialArray object specifying one ConnectorPotential object for each force potential contribution. This member can be specified only if frictionModel = USER_CUSTOMIZED, and if slipStyle = COMPUTE.

  • table (tuple, default: ()) – A sequence of sequences of Floats specifying friction properties. The default value is an empty sequence.If frictionModel = PREDEFINED, each sequence of the table data specifies:If applicable, the first geometric scaling constant relevant to frictional interactions.Etc., up to as many geometric scaling constants as are associated with this connection type.Internal contact force/moment generating friction in the first predefined slip direction.If applicable, internal contact force/moment generating friction in the second predefined slip direction.Connector constitutive relative motion in the direction specified by independentComponent.Accumulated slip in the first predefined slip direction, if the data depend on accumulated slip.Temperature, if the data depend on temperature.Value of the first field variable, if the data depend on field variables.Value of the second field variable.Etc.If frictionModel = USER_CUSTOMIZED, each sequence of the table data specifies:Effective radius of the cylindrical or spherical surface over which frictional slip occurs in the connector associated with frictional effects in the direction specified by tangentDirection. This radius is relevant only if the connection type includes an available rotational component of relative motion and tangentDirection = SLIP_DIRECTION.Internal contact force/moment generating friction in the direction specified by tangentDirection.Connector constitutive relative motion in the direction specified by independentComponent.Accumulated slip in the direction specified by tangentDirection, if the data depend on accumulated slip.Temperature, if the data depend on temperature.Value of the first field variable, if the data depend on field variables.Value of the second field variable.Etc.

  • independentComponents (tuple, default: ()) – A sequence of Ints specifying the independent components. Possible values are 1 ≤ independentComponents ≤ 6. In addition, each independent component value must be unique. The independentComponents argument applies only if frictionModel = USER_CUSTOMIZED. Only available components can be specified. The default value is an empty sequence.

Returns:

A ConnectorFriction object.

Return type:

ConnectorFriction

Raises:

ValueError –

ConnectorLock(lockingComponent=abaqusConstants.ALL, minMotion=None, maxMotion=None, minForce=None, maxForce=None, components=())[source]#

This method creates a connector lock behavior option for a ConnectorSection.

Note

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorLock
import odbConnectorBehavior
odbConnectorBehavior.ConnectorLock

Note

Check ConnectorLock on help.3ds.com/0.1..

Parameters:

  • lockingComponent (SymbolicConstant, default: ALL) – The SymbolicConstant ALL or an Int specifying the motion components that are locked. If an Int is specified, only that motion component is locked when the locking criteria are satisfied. If lockingComponent = ALL, all motion components are locked. The default value is ALL.

  • minMotion (Optional[float], default: None) – None or a Float specifying the lower bound for the connector’s relative position for all specified components, or no lower bound. The default value is None.

  • maxMotion (Optional[float], default: None) – None or a Float specifying the upper bound for the connector’s relative position for all specified components, or no upper bound. The default value is None.

  • minForce (Optional[float], default: None) – None or a Float specifying the lower bound of the force or moment in the directions of the specified components at which locking occurs, or no lower bound. The default value is None.

  • maxForce (Optional[float], default: None) – None or a Float specifying the upper bound of the force or moment in the directions of the specified components at which locking occurs, or no upper bound. The default value is None.

  • components (tuple, default: ()) – A sequence of Ints specifying the components of relative motion for which the behavior is defined. Possible values are 1 ≤ components ≤ 6. Only available components can be specified. The default value is an empty sequence.

Returns:

A ConnectorLock object.

Return type:

ConnectorLock

Raises:

ValueError –

ConnectorPlasticity(coupling=abaqusConstants.UNCOUPLED, isotropic=ON, isotropicType=abaqusConstants.TABULAR, isotropicTemperature=OFF, isotropicDependencies=0, kinematic=OFF, kinematicType=abaqusConstants.HALF_CYCLE, kinematicTemperature=OFF, kinematicDependencies=0, forcePotentialOperator=abaqusConstants.SUM, forcePotentialExponent=2, connectorPotentials=None, isotropicTable=(), kinematicTable=(), components=())[source]#

This method creates a connector plasticity behavior option for a ConnectorSection object.

Note

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorPlasticity
import odbConnectorBehavior
odbConnectorBehavior.ConnectorPlasticity

Note

Check ConnectorPlasticity on help.3ds.com/0.1..

Parameters:

  • coupling (SymbolicConstant, default: UNCOUPLED) – A SymbolicConstant specifying whether or not the behavior is coupled. Possible values are UNCOUPLED and COUPLED. The default value is UNCOUPLED.

  • isotropic (Union[AbaqusBoolean, bool], default: ON) – A Boolean specifying whether isotropic hardening data will be used. The default value is ON.If isotropic = OFF, then kinematic must be specified as ON.

  • isotropicType (SymbolicConstant, default: TABULAR) – A SymbolicConstant specifying the type of isotropic hardening to be specified. Possible values are TABULAR and EXPONENTIAL_LAW. The default value is TABULAR.This argument is applicable only if isotropic = ON.

  • isotropicTemperature (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the isotropic data depend on temperature. The default value is OFF.This argument is applicable only if isotropic = ON.

  • isotropicDependencies (int, default: 0) – An Int specifying the number of field variable dependencies for the isotropic data. The default value is 0.This argument is applicable only if isotropic = ON.

  • kinematic (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether kinematic hardening data will be used. The default value is OFF.If kinematic = OFF, then isotropic must be specified as ON.

  • kinematicType (SymbolicConstant, default: HALF_CYCLE) – A SymbolicConstant specifying the type of kinematic hardening to be specified. Possible values are HALF_CYCLE, STABILIZED, and PARAMETERS. The default value is HALF_CYCLE.This argument is applicable only if kinematic = ON.

  • kinematicTemperature (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the kinematic data depend on temperature. The default value is OFF.This argument is applicable only if kinematic = ON.

  • kinematicDependencies (int, default: 0) – An Int specifying the number of field variable dependencies for the kinematic data. The default value is 0.This argument is applicable only if kinematic = ON.

  • forcePotentialOperator (SymbolicConstant, default: SUM) – A SymbolicConstant specifying the contribution operator for the force potential contributions. Possible values are SUM and MAXIMUM. The default value is SUM.This argument is applicable only if coupling = COUPLED.

  • forcePotentialExponent (float, default: 2) – A Float specifying the number equal to the inverse of the overall exponent in the force potential definition. The default value is 2.0.This argument is applicable only if coupling = COUPLED and if forcePotentialOperator = SUM.

  • connectorPotentials (Optional[List[ConnectorPotential]], default: None) – A ConnectorPotentialArray object specifying one ConnectorPotential object for each force potential contribution. This member can be specified only if coupling = COUPLED.

  • isotropicTable (tuple, default: ()) – A sequence of sequences of Floats specifying isotropic plasticity properties. Items in the isotropicTable data are described below. This argument is applicable only if isotropic = ON. The default value is an empty sequence.

  • kinematicTable (tuple, default: ()) – A sequence of sequences of Floats specifying kinematic plasticity properties. Items in the kinematicTable data are described below. This argument is applicable only if kinematic = ON. The default value is an empty sequence.

  • components (tuple, default: ()) – A sequence of Ints specifying the components of relative motion for which the behavior is defined. Possible values are 1 ≤ components ≤ 6. Only available components can be specified. This argument can be specified only if coupling = UNCOUPLED. The default value is an empty sequence.

Returns:

A ConnectorPlasticity object.

Return type:

ConnectorPlasticity

Raises:

ValueError –

ConnectorPotential(componentStyle=abaqusConstants.COMPONENT_NUMBER, componentNumber=0, sign=abaqusConstants.POSITIVE, scaleFactor=1, positiveExponent=2, shiftFactor=0, hFunction=abaqusConstants.ABS)[source]#

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

Note

This function can be accessed by:

mdb.models[name].sections[name].behaviorOptions[i].ConnectorPotential
session.odbs[name].sections[name].behaviorOptions[i].ConnectorPotential

Note

Check ConnectorPotential on help.3ds.com/0.1..

Parameters:

  • componentStyle (SymbolicConstant, default: COMPONENT_NUMBER) – A SymbolicConstant specifying whether a component number or the name of the DerivedComponent object will be used in the contribution. Possible values are COMPONENT_NUMBER and DERIVED_COMPONENT. The default value is COMPONENT_NUMBER.

  • componentNumber (int, default: 0) – An Int specifying the component number used in the contribution. This argument is applicable only if componentStyle = COMPONENT_NUMBER. Possible values are 1 ≤ componentNumber ≤ 6. Only available components can be specified. The default value is 0.

  • sign (SymbolicConstant, default: POSITIVE) – A SymbolicConstant specifying the sign of the contribution. Possible values are POSITIVE and NEGATIVE. The default value is POSITIVE.

  • scaleFactor (float, default: 1) – A Float specifying the scaling factor for the contribution. The default value is 1.0.

  • positiveExponent (float, default: 2) – A Float specifying the positive exponent for the contribution. The default value is 2.0.This argument is ignored if the potential operator of the invoking behavior option is set to MAXIMUM.

  • shiftFactor (float, default: 0) – A Float specifying the shift factor for the contribution. The default value is 0.0.

  • hFunction (SymbolicConstant, default: ABS) – A SymbolicConstant specifying the H function of the contribution: either absolute value, Macauley bracket, or the identity function. Possible values are ABS, MACAULEY, and IDENTITY. The default value is ABS.The value of IDENTITY can be used only if positiveExponent = 1.0 and the potential exponent of the invoking behavior option is also 1.0 (i.e., the potential operator of the invoking behavior option must be SUM).

Returns:

A ConnectorPotential object.

Return type:

ConnectorPotential

Raises:

ValueError –

ConnectorStop(minMotion=None, maxMotion=None, components=())[source]#

This method creates a connector stop behavior option for a ConnectorSection object.

Note

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorStop
import odbConnectorBehavior
odbConnectorBehavior.ConnectorStop

Note

Check ConnectorStop on help.3ds.com/0.1..

Parameters:

  • minMotion (Optional[float], default: None) – None or a Float specifying the lower bound for the connector’s relative position for all specified components, or no lower bound. The default value is None.

  • maxMotion (Optional[float], default: None) – None or a Float specifying the upper bound for the connector’s relative position for all specified components, or no upper bound. The default value is None.

  • components (tuple, default: ()) – A sequence of Ints specifying the components of relative motion for which the behavior is defined. Possible values are 1 ≤ components ≤ 6. Only available components can be specified. The default value is an empty sequence.

Returns:

A ConnectorStop object.

Return type:

ConnectorStop

Raises:

ValueError –

DerivedComponent()[source]#

This method creates a DerivedComponent object.

Note

This function can be accessed by:

mdb.models[name].sections[name].behaviorOptions[i].connectorPotentials[i].DerivedComponent
mdb.models[name].sections[name].behaviorOptions[i].DerivedComponent
mdb.models[name].sections[name].behaviorOptions[i].evolutionPotentials[i].DerivedComponent
mdb.models[name].sections[name].behaviorOptions[i].initiationPotentials[i].DerivedComponent
session.odbs[name].sections[name].behaviorOptions[i].connectorPotentials[i].DerivedComponent
session.odbs[name].sections[name].behaviorOptions[i].DerivedComponent
session.odbs[name].sections[name].behaviorOptions[i].evolutionPotentials[i].DerivedComponent
session.odbs[name].sections[name].behaviorOptions[i].initiationPotentials[i].DerivedComponent
Returns:

A DerivedComponent object.

Return type:

DerivedComponent

Raises:

ValueError –

TangentialBehavior(formulation=abaqusConstants.PENALTY, slipRateDependency=OFF, pressureDependency=OFF, temperatureDependency=OFF, dependencies=0, exponentialDecayDefinition=abaqusConstants.COEFFICIENTS, shearStressLimit=None, maximumElasticSlip=abaqusConstants.FRACTION, fraction=None, absoluteDistance=None, table=())[source]#

This method creates a TangentialBehavior object.

Note

This function can be accessed by:

mdb.models[name].sections[name].behaviorOptions[i].TangentialBehavior
session.odbs[name].sections[name].behaviorOptions[i].TangentialBehavior

Note

Check TangentialBehavior on help.3ds.com/0.1..

Parameters:

  • formulation (SymbolicConstant, default: PENALTY) – A SymbolicConstant specifying the friction coefficient formulation. Possible values are PENALTY and EXPONENTIAL_DECAY. The default value is PENALTY.

  • slipRateDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the data depend on slip rate. The default value is OFF.

  • pressureDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the data depend on contact pressure. The default value is OFF.

  • temperatureDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the data depend on temperature. The default value is OFF.

  • dependencies (int, default: 0) – An Int specifying the number of field variables for the data. The default value is 0.

  • exponentialDecayDefinition (SymbolicConstant, default: COEFFICIENTS) – A SymbolicConstant specifying the exponential decay definition for the data. Possible values are COEFFICIENTS and TEST_DATA. The default value is COEFFICIENTS.

  • shearStressLimit (Optional[float], default: None) – None or a Float specifying no upper limit or the friction coefficient shear stress limit. The default value is None.

  • maximumElasticSlip (SymbolicConstant, default: FRACTION) – A SymbolicConstant specifying the method for modifying the allowable elastic slip. Possible values are FRACTION and ABSOLUTE_DISTANCE. The default value is FRACTION.This argument applies only to Abaqus/Standard analyses.

  • fraction (Optional[float], default: None) – A Float specifying the ratio of the allowable maximum elastic slip to a characteristic model dimension. The default value is 10-4.This argument applies only to Abaqus/Standard analyses.

  • absoluteDistance (Optional[float], default: None) – None or a Float specifying the absolute magnitude of the allowable elastic slip. The default value is None.This argument applies only to Abaqus/Standard analyses.

  • table (tuple, default: ()) – A sequence of sequences of Floats specifying the tangential properties. Items in the table data are described below. The default value is an empty sequence.

Returns:

A TangentialBehavior object. .

Return type:

TangentialBehavior

TransverseShearBeam(scfDefinition, k23=None, k13=None, slendernessCompensation=0)[source]#

This method creates a TransverseShearBeam object.

Note

This function can be accessed by:

mdb.models[name].sections[name].TransverseShearBeam
session.odbs[name].sections[name].TransverseShearBeam

Note

Check TransverseShearBeam on help.3ds.com/0.1..

Parameters:

  • scfDefinition (SymbolicConstant) – A SymbolicConstant specifying how slenderness compensation factor of the section is given. Possible values are ANALYSIS_DEFAULT, COMPUTED, and VALUE.

  • k23 (Optional[float], default: None) – None or a Float specifying the k23 shear stiffness of the section. The default value is None.

  • k13 (Optional[float], default: None) – None or a Float specifying the k13 shear stiffness of the section. The default value is None.

  • slendernessCompensation (Union[SymbolicConstant, float], default: 0) – The SymbolicConstant COMPUTED or a Float specifying the slenderness compensation factor of the section. The default value is 0.25.

Returns:

A TransverseShearBeam object.

Return type:

TransverseShearBeam

TransverseShearShell(k11, k22, k12)[source]#

This method creates a TransverseShearShell object.

Note

This function can be accessed by:

mdb.models[name].sections[name].TransverseShearShell
session.odbs[name].sections[name].TransverseShearShell

Note

Check TransverseShearShell on help.3ds.com/0.1..

Parameters:

  • k11 (float) – A Float specifying the shear stiffness of the section in the first direction.

  • k22 (float) – A Float specifying the shear stiffness of the section in the second direction.

  • k12 (float) – A Float specifying the coupling term in the shear stiffness of the section.

Returns:

A TransverseShearShell object.

Return type:

TransverseShearShell

beamTransverseShear: TransverseShearBeam = <abaqus.Section.TransverseShearBeam.TransverseShearBeam object>[source]#

A TransverseShearBeam object.

behaviorOptions: ConnectorBehaviorOptionArray = [][source]#

A ConnectorBehaviorOptionArray object.

name: str = ''[source]#

A String specifying the repository key.

sectionsFromOdb(fileName)[source]#

This method creates Section objects by reading an output database. The new sections are placed in the sections repository.

Note

This function can be accessed by:

mdb.models[name].sectionsFromOdb

Note

Check SectionBase.sectionsFromOdb on help.3ds.com/0.1..

Parameters:

fileName (str) – A String specifying the name of the output database file (including the .odb extension) to be read. This String can also be the full path to the output database file if it is located in another directory.

Returns:

A list of Section objects.

Return type:

List[Section]

transverseShear: TransverseShearShell = <abaqus.Section.TransverseShearShell.TransverseShearShell object>[source]#

A TransverseShearShell object.

SectionBase#

class SectionBase[source]#

The Section object defines the properties of a section. The Section object is the abstract base type for other Section objects. The Section object has no explicit constructor. The methods and members of the Section object are common to all objects derived from the Section.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

Note

Check SectionBase on help.3ds.com/0.1..

Public Data Attributes:

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
beamTransverseShear: TransverseShearBeam = <abaqus.Section.TransverseShearBeam.TransverseShearBeam object>[source]#

A TransverseShearBeam object.

behaviorOptions: List[ConnectorBehaviorOption] = [][source]#

A ConnectorBehaviorOptionArray object.

name: str = ''[source]#

A String specifying the repository key.

sectionsFromOdb(fileName)[source]#

This method creates Section objects by reading an output database. The new sections are placed in the sections repository.

Note

This function can be accessed by:

mdb.models[name].sectionsFromOdb

Note

Check SectionBase.sectionsFromOdb on help.3ds.com/0.1..

Parameters:

fileName (str) – A String specifying the name of the output database file (including the .odb extension) to be read. This String can also be the full path to the output database file if it is located in another directory.

Returns:

A list of Section objects.

Return type:

List[Section]

transverseShear: TransverseShearShell = <abaqus.Section.TransverseShearShell.TransverseShearShell object>[source]#

A TransverseShearShell object.

AcousticInfiniteSection#

class AcousticInfiniteSection(name, material, thickness=1, order=10)[source]#

The AcousticInfiniteSection object defines the properties of an acoustic section. The AcousticInfiniteSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • SOLID SECTION

Note

Check AcousticInfiniteSection on help.3ds.com/0.1..

Public Data Attributes:

thickness

A Float specifying the thickness of the section.

order

An Int specifying the number of ninth-order polynomials that will be used to resolve the variation of the acoustic field in the infinite direction.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

__init__(name, material[, thickness, order])

This method creates an AcousticInfiniteSection object.

setValues([thickness, order])

This method modifies the AcousticInfiniteSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
material: str[source]#

A String specifying the name of the material.

order: int = 10[source]#

An Int specifying the number of ninth-order polynomials that will be used to resolve the variation of the acoustic field in the infinite direction. Possible values are 0 << order ≤ 10. The default value is 10.

setValues(thickness=1, order=10)[source]#

This method modifies the AcousticInfiniteSection object.

Note

Check AcousticInfiniteSection.setValues on help.3ds.com/0.1..

Parameters:

  • thickness (float, default: 1) – A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

  • order (int, default: 10) – An Int specifying the number of ninth-order polynomials that will be used to resolve the variation of the acoustic field in the infinite direction. Possible values are 0 << order ≤ 10. The default value is 10.

Raises:

RangeError –

thickness: float = 1[source]#

A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

AcousticInterfaceSection#

class AcousticInterfaceSection(name, thickness=1)[source]#

The AcousticInterfaceSection object defines the properties of an acoustic section. The AcousticInterfaceSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • INTERFACE

Note

Check AcousticInterfaceSection on help.3ds.com/0.1..

Public Data Attributes:

thickness

A Float specifying the thickness of the section.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

__init__(name[, thickness])

This method creates an AcousticInterfaceSection object.

setValues([thickness])

This method modifies the AcousticInterfaceSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
setValues(thickness=1)[source]#

This method modifies the AcousticInterfaceSection object.

Note

Check AcousticInterfaceSection.setValues on help.3ds.com/0.1..

Parameters:

thickness (float, default: 1) – A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

Raises:

RangeError –

thickness: float = 1[source]#

A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

BeamSection#

class BeamSection(name, integration, profile, poissonRatio=0, thermalExpansion=OFF, temperatureDependency=OFF, dependencies=0, density=None, referenceTemperature=None, temperatureVar=abaqusConstants.LINEAR, alphaDamping=0, betaDamping=0, compositeDamping=0, useFluidInertia=OFF, submerged=abaqusConstants.FULLY, fluidMassDensity=None, crossSectionRadius=None, lateralMassCoef=1, axialMassCoef=0, massOffsetX=0, massOffsetY=0, beamShape=abaqusConstants.CONSTANT, material='', table=(), outputPts=(), centroid=(0.0, 0.0), shearCenter=(0.0, 0.0), profileEnd='')[source]#

The BeamSection object defines the properties of a beam section. The BeamSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The table data for this object are:

  • E, the Young’s modulus of the section.

  • G, the torsional shear modulus of the section.

  • Thermal expansion coefficient, if using thermal expansion.

  • Temperature, if the data depend on temperature.

  • Value of the first field variable, if the data depend on field variables.

  • Value of the second field variable.

  • Etc.

The corresponding analysis keywords are:

  • BEAM GENERAL SECTION

  • BEAM SECTION

  • BEAM FLUID INERTIA

  • CENTROID

  • DAMPING

  • SHEAR CENTER

  • SECTION POINTS

Note

Check BeamSection on help.3ds.com/0.1..

Public Data Attributes:

beamTransverseShear

A TransverseShearBeam object specifying the transverse shear stiffness properties.

poissonRatio

A Float specifying the Poisson's ratio of the section.

thermalExpansion

A Boolean specifying whether to use thermal expansion data.

temperatureDependency

A Boolean specifying whether the data depend on temperature.

dependencies

An Int specifying the number of field variable dependencies.

density

None or a Float specifying the density of the section.

referenceTemperature

None or a Float specifying the reference temperature of the section.

temperatureVar

A SymbolicConstant specifying the temperature variation for the section.

alphaDamping

A Float specifying the αRαR factor to create mass proportional damping in direct-integration dynamics.

betaDamping

A Float specifying the βRβR factor to create stiffness proportional damping in direct-integration dynamics.

compositeDamping

A Float specifying the fraction of critical damping to be used in calculating composite damping factors for the modes (for use in modal dynamics).

useFluidInertia

A Boolean specifying whether added mass effects will be simulated.

submerged

A SymbolicConstant specifying whether the section is either full submerged or half submerged.

fluidMassDensity

None or a Float specifying the mass density of the fluid.

crossSectionRadius

None or a Float specifying the radius of the cylindrical cross-section.

lateralMassCoef

A Float specifying the added mass coefficient, CACA, for lateral motions of the beam.

axialMassCoef

A Float specifying the added mass coefficient, C(A−E)C(A-E), for motions along the axis of the beam.

massOffsetX

A Float specifying the local 1-coordinate of the center of the cylindrical cross-section with respect to the beam cross-section.

massOffsetY

A Float specifying the local 2-coordinate of the center of the cylindrical cross-section with respect to the beam cross-section.

beamShape

A SymbolicConstant specifying the change in cross-section of the beam along length.

material

A String specifying the name of the material.

table

A sequence of sequences of Floats specifying the items described below.

outputPts

A sequence of pairs of Floats specifying the positions at which output is requested.

centroid

A pair of Floats specifying the X - Y coordinates of the centroid.

shearCenter

A pair of Floats specifying the X - Y coordinates of the shear center.

profileEnd

A String specifying the name of the end profile.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object specifying the transverse shear stiffness properties.

transverseShear

A TransverseShearShell object.

Public Methods:

__init__(name, integration, profile[, ...])

This method creates a BeamSection object.

setValues([poissonRatio, thermalExpansion, ...])

This method modifies the BeamSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
alphaDamping: float = 0[source]#

A Float specifying the αRαR factor to create mass proportional damping in direct-integration dynamics. The default value is 0.0.

axialMassCoef: float = 0[source]#

A Float specifying the added mass coefficient, C(A−E)C(A-E), for motions along the axis of the beam. This argument affects only the term added to the free end(s) of the beam, and applies only when useFluidInertia = True. The default value is 0.0.

beamShape: Literal[CONSTANT, TAPERED] = CONSTANT[source]#

A SymbolicConstant specifying the change in cross-section of the beam along length. Possible values are CONSTANT and TAPERED. The default value is CONSTANT. This parameter is available for manipulating the model database but not for the ODB API.

beamTransverseShear: TransverseShearBeam = <abaqus.Section.TransverseShearBeam.TransverseShearBeam object>[source]#

A TransverseShearBeam object specifying the transverse shear stiffness properties.

betaDamping: float = 0[source]#

A Float specifying the βRβR factor to create stiffness proportional damping in direct-integration dynamics. The default value is 0.0.

centroid: Tuple[float, float] = (0.0, 0.0)[source]#

A pair of Floats specifying the X - Y coordinates of the centroid. The default value is (0.0, 0.0).

compositeDamping: float = 0[source]#

A Float specifying the fraction of critical damping to be used in calculating composite damping factors for the modes (for use in modal dynamics). The default value is 0.0.

crossSectionRadius: Optional[float] = None[source]#

None or a Float specifying the radius of the cylindrical cross-section. This argument applies only when useFluidInertia = True and must be specified in that case. The default value is None.

density: Optional[float] = None[source]#

None or a Float specifying the density of the section. The default value is None.

dependencies: int = 0[source]#

An Int specifying the number of field variable dependencies. The default value is 0.

fluidMassDensity: Optional[float] = None[source]#

None or a Float specifying the mass density of the fluid. This argument applies only when useFluidInertia = True and must be specified in that case. The default value is None.

integration: Literal[BEFORE_ANALYSIS, DURING_ANALYSIS][source]#

A SymbolicConstant specifying the integration method for the section. Possible values are BEFORE_ANALYSIS and DURING_ANALYSIS.

lateralMassCoef: float = 1[source]#

A Float specifying the added mass coefficient, CACA, for lateral motions of the beam. This argument applies only when*useFluidInertia* = True. The default value is 1.0.

massOffsetX: float = 0[source]#

A Float specifying the local 1-coordinate of the center of the cylindrical cross-section with respect to the beam cross-section. This argument applies only when useFluidInertia = True. The default value is 0.0.

massOffsetY: float = 0[source]#

A Float specifying the local 2-coordinate of the center of the cylindrical cross-section with respect to the beam cross-section. This argument applies only when useFluidInertia = True. The default value is 0.0.

material: str = ''[source]#

A String specifying the name of the material. The default value is an empty string. The material is required when integration is “DURING_ANALYSIS”.

outputPts: tuple = ()[source]#

A sequence of pairs of Floats specifying the positions at which output is requested. The default value is an empty sequence.

poissonRatio: float = 0[source]#

A Float specifying the Poisson’s ratio of the section. The default value is 0.0.

profile: str[source]#

A String specifying the name of the profile. This argument represents the start profile in case of beamShape = TAPERED.

profileEnd: str = ''[source]#

A String specifying the name of the end profile. The type of the end profile must be same as that of the start profile. This argument is valid only when beamShape = TAPERED. The default value is an empty string. This parameter is available for manipulating the model database but not for the ODB API.

referenceTemperature: Optional[float] = None[source]#

None or a Float specifying the reference temperature of the section. The default value is None.

setValues(poissonRatio=0, thermalExpansion=OFF, temperatureDependency=OFF, dependencies=0, density=None, referenceTemperature=None, temperatureVar=abaqusConstants.LINEAR, alphaDamping=0, betaDamping=0, compositeDamping=0, useFluidInertia=OFF, submerged=abaqusConstants.FULLY, fluidMassDensity=None, crossSectionRadius=None, lateralMassCoef=1, axialMassCoef=0, massOffsetX=0, massOffsetY=0, beamShape=abaqusConstants.CONSTANT, material='', table=(), outputPts=(), centroid=(0.0, 0.0), shearCenter=(0.0, 0.0), profileEnd='')[source]#

This method modifies the BeamSection object.

Note

Check BeamSection.setValues on help.3ds.com/0.1..

Parameters:

  • poissonRatio (float, default: 0) – A Float specifying the Poisson’s ratio of the section. The default value is 0.0.

  • thermalExpansion (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether to use thermal expansion data. The default value is OFF.

  • temperatureDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the data depend on temperature. The default value is OFF.

  • dependencies (int, default: 0) – An Int specifying the number of field variable dependencies. The default value is 0.

  • density (Optional[float], default: None) – None or a Float specifying the density of the section. The default value is None.

  • referenceTemperature (Optional[float], default: None) – None or a Float specifying the reference temperature of the section. The default value is None.

  • temperatureVar (Literal[LINEAR, INTERPOLATED], default: LINEAR) – A SymbolicConstant specifying the temperature variation for the section. Possible values are LINEAR and INTERPOLATED. The default value is LINEAR.

  • alphaDamping (float, default: 0) – A Float specifying the αRαR factor to create mass proportional damping in direct-integration dynamics. The default value is 0.0.

  • betaDamping (float, default: 0) – A Float specifying the βRβR factor to create stiffness proportional damping in direct-integration dynamics. The default value is 0.0.

  • compositeDamping (float, default: 0) – A Float specifying the fraction of critical damping to be used in calculating composite damping factors for the modes (for use in modal dynamics). The default value is 0.0.

  • useFluidInertia (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether added mass effects will be simulated. The default value is OFF.

  • submerged (Literal[FULLY, HALF], default: FULLY) – A SymbolicConstant specifying whether the section is either full submerged or half submerged. This argument applies only when useFluidInertia = True. Possible values are FULLY and HALF. The default value is FULLY.

  • fluidMassDensity (Optional[float], default: None) – None or a Float specifying the mass density of the fluid. This argument applies only when useFluidInertia = True and must be specified in that case. The default value is None.

  • crossSectionRadius (Optional[float], default: None) – None or a Float specifying the radius of the cylindrical cross-section. This argument applies only when useFluidInertia = True and must be specified in that case. The default value is None.

  • lateralMassCoef (float, default: 1) – A Float specifying the added mass coefficient, CACA, for lateral motions of the beam. This argument applies only when*useFluidInertia* = True. The default value is 1.0.

  • axialMassCoef (float, default: 0) – A Float specifying the added mass coefficient, C(A−E)C(A-E), for motions along the axis of the beam. This argument affects only the term added to the free end(s) of the beam, and applies only when useFluidInertia = True. The default value is 0.0.

  • massOffsetX (float, default: 0) – A Float specifying the local 1-coordinate of the center of the cylindrical cross-section with respect to the beam cross-section. This argument applies only when useFluidInertia = True. The default value is 0.0.

  • massOffsetY (float, default: 0) – A Float specifying the local 2-coordinate of the center of the cylindrical cross-section with respect to the beam cross-section. This argument applies only when useFluidInertia = True. The default value is 0.0.

  • beamShape (Literal[CONSTANT, TAPERED], default: CONSTANT) – A SymbolicConstant specifying the change in cross-section of the beam along length. Possible values are CONSTANT and TAPERED. The default value is CONSTANT. This parameter is available for manipulating the model database but not for the ODB API.

  • material (str, default: '') – A String specifying the name of the material. The default value is an empty string. The material is required when integration is “DURING_ANALYSIS”.

  • table (tuple, default: ()) – A sequence of sequences of Floats specifying the items described below. The default value is an empty sequence.

  • outputPts (tuple, default: ()) – A sequence of pairs of Floats specifying the positions at which output is requested. The default value is an empty sequence.

  • centroid (Tuple[float, float], default: (0.0, 0.0)) – A pair of Floats specifying the X - Y coordinates of the centroid. The default value is (0.0, 0.0).

  • shearCenter (Tuple[float, float], default: (0.0, 0.0)) – A pair of Floats specifying the X - Y coordinates of the shear center. The default value is (0.0, 0.0).

  • profileEnd (str, default: '') – A String specifying the name of the end profile. The type of the end profile must be same as that of the start profile. This argument is valid only when beamShape = TAPERED. The default value is an empty string. This parameter is available for manipulating the model database but not for the ODB API.

shearCenter: Tuple[float, float] = (0.0, 0.0)[source]#

A pair of Floats specifying the X - Y coordinates of the shear center. The default value is (0.0, 0.0).

submerged: Literal[FULLY, HALF] = FULLY[source]#

A SymbolicConstant specifying whether the section is either full submerged or half submerged. This argument applies only when useFluidInertia = True. Possible values are FULLY and HALF. The default value is FULLY.

table: tuple = ()[source]#

A sequence of sequences of Floats specifying the items described below. The default value is an empty sequence.

temperatureDependency: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether the data depend on temperature. The default value is OFF.

temperatureVar: Literal[LINEAR, INTERPOLATED] = LINEAR[source]#

A SymbolicConstant specifying the temperature variation for the section. Possible values are LINEAR and INTERPOLATED. The default value is LINEAR.

thermalExpansion: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether to use thermal expansion data. The default value is OFF.

useFluidInertia: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether added mass effects will be simulated. The default value is OFF.

CohesiveSection#

class CohesiveSection(name, response, material, initialThicknessType=abaqusConstants.SOLVER_DEFAULT, initialThickness=1, outOfPlaneThickness=None)[source]#

The CohesiveSection object defines the properties of a cohesive section. The CohesiveSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • COHESIVE SECTION

Note

Check CohesiveSection on help.3ds.com/0.1..

Public Data Attributes:

initialThicknessType

A SymbolicConstant specifying the method used to compute the initial thickness.

initialThickness

A Float specifying the initial thickness for the section.

outOfPlaneThickness

None or a Float specifying the out-of-plane thickness for the section.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

__init__(name, response, material[, ...])

This method creates a CohesiveSection object.

setValues([initialThicknessType, ...])

This method modifies the CohesiveSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
initialThickness: float = 1[source]#

A Float specifying the initial thickness for the section. The initialThickness argument applies only when initialThicknessType = SPECIFY. The default value is 1.0.

initialThicknessType: Literal[SOLVER_DEFAULT, GEOMETRY, SPECIFY] = SOLVER_DEFAULT[source]#

A SymbolicConstant specifying the method used to compute the initial thickness. Possible values are: SOLVER_DEFAULT, specifying that Abaqus will use the analysis product default; GEOMETRY, specifying that Abaqus will compute the thickness from the nodal coordinates of the elements. SPECIFY, specifying that Abaqus will use the value given for initialThickness The default value is SOLVER_DEFAULT.

material: str[source]#

A String specifying the name of the material.

outOfPlaneThickness: Optional[float] = None[source]#

None or a Float specifying the out-of-plane thickness for the section. The default value is None.

response: Literal[TRACTION_SEPARATION, CONTINUUM, GASKET][source]#

A SymbolicConstant specifying the geometric assumption that defines the constitutive behavior of the cohesive elements. Possible values are TRACTION_SEPARATION, CONTINUUM, and GASKET.

setValues(initialThicknessType=abaqusConstants.SOLVER_DEFAULT, initialThickness=1, outOfPlaneThickness=None)[source]#

This method modifies the CohesiveSection object.

Note

Check CohesiveSection.setValues on help.3ds.com/0.1..

Parameters:

  • initialThicknessType (Literal[SOLVER_DEFAULT, GEOMETRY, SPECIFY], default: SOLVER_DEFAULT) – A SymbolicConstant specifying the method used to compute the initial thickness. Possible values are:SOLVER_DEFAULT, specifying that Abaqus will use the analysis product defaultGEOMETRY, specifying that Abaqus will compute the thickness from the nodal coordinates of the elements.SPECIFY, specifying that Abaqus will use the value given for initialThickness The default value is SOLVER_DEFAULT.

  • initialThickness (float, default: 1) – A Float specifying the initial thickness for the section. The initialThickness argument applies only when initialThicknessType = SPECIFY. The default value is 1.0.

  • outOfPlaneThickness (Optional[float], default: None) – None or a Float specifying the out-of-plane thickness for the section. The default value is None.

Raises:

RangeError –

CompositeShellSection#

class CompositeShellSection(name, layup, symmetric=OFF, thicknessType=abaqusConstants.UNIFORM, preIntegrate=OFF, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, integrationRule=abaqusConstants.SIMPSON, temperature=abaqusConstants.GRADIENT, idealization=abaqusConstants.NO_IDEALIZATION, nTemp=None, thicknessModulus=None, useDensity=OFF, density=0, layupName='', thicknessField='', nodalThicknessField='')[source]#

The CompositeShellSection object defines the properties of a composite shell section. The CompositeShellSection object is derived from the GeometryShellSection object.

Note

This object can be accessed by:

import section
mdb.models[name].parts[name].compositeLayups[i].section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • SHELL SECTION

  • SHELL GENERAL SECTION

Note

Check CompositeShellSection on help.3ds.com/0.1..

Public Data Attributes:

rebarLayers

A RebarLayers object specifying reinforcement properties.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.

symmetric

A Boolean specifying whether or not the layup should be made symmetric by the analysis.

thicknessType

A SymbolicConstant specifying the distribution used for defining the thickness of the elements.

preIntegrate

A Boolean specifying whether the shell section properties are specified by the user prior to the analysis (ON) or integrated during the analysis (OFF).

poissonDefinition

A SymbolicConstant specifying whether to use the default value for the Poisson's ratio.

poisson

A Float specifying the Poisson's ratio.

integrationRule

A SymbolicConstant specifying the shell section integration rule.

temperature

A SymbolicConstant specifying the mode used for temperature and field variable input across the section thickness.

idealization

A SymbolicConstant specifying the mechanical idealization used for the section calculations.

nTemp

None or an Int specifying the number of temperature points to be input.

thicknessModulus

None or a Float specifying the effective thickness modulus.

useDensity

A Boolean specifying whether or not to use the value of density.

density

A Float specifying the value of density to apply to this section.

layupName

A String specifying the layup name for this section.

thicknessField

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements.

nodalThicknessField

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements at each node.
Inherited from GeometryShellSection

name

A String specifying the repository key.

thicknessType

A SymbolicConstant specifying the distribution used for defining the thickness of the elements.

preIntegrate

A Boolean specifying whether the shell section properties are specified by the user prior to the analysis (ON) or integrated during the analysis (OFF).

poissonDefinition

A SymbolicConstant specifying whether to use the default value for the Poisson's ratio.

poisson

A Float specifying the Poisson's ratio.

integrationRule

A SymbolicConstant specifying the shell section integration rule.

temperature

A SymbolicConstant specifying the mode used for temperature and field variable input across the section thickness.

idealization

A SymbolicConstant specifying the mechanical idealization used for the section calculations.

nTemp

None or an Int specifying the number of temperature points to be input.

thicknessModulus

None or a Float specifying the effective thickness modulus.

useDensity

A Boolean specifying whether or not to use the value of density.

density

A Float specifying the value of density to apply to this section.

thicknessField

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements.

rebarLayers

A RebarLayers object specifying reinforcement properties.

nodalThicknessField

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements at each node.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.
Inherited from ShellSection

name

A String specifying the repository key.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.

Public Methods:

__init__(name, layup[, symmetric, ...])

This method creates a CompositeShellSection object.

setValues([symmetric, thicknessType, ...])

This method modifies the CompositeShellSection object.
Inherited from GeometryShellSection

__init__(name, layup[, symmetric, ...])

This method creates a CompositeShellSection object.

RebarLayers(rebarSpacing, layerTable)

This method creates a RebarLayers object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
density: float = 0[source]#

A Float specifying the value of density to apply to this section. The default value is 0.0.

idealization: Literal[NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, BENDING] = NO_IDEALIZATION[source]#

A SymbolicConstant specifying the mechanical idealization used for the section calculations. This member is only applicable when preIntegrate is set to ON. Possible values are NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, and BENDING. The default value is NO_IDEALIZATION.

integrationRule: Literal[SIMPSON, GAUSS] = SIMPSON[source]#

A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.

layup: List[SectionLayer][source]#

A SectionLayerArray object specifying the shell cross-section.

layupName: str = ''[source]#

A String specifying the layup name for this section. The default value is an empty string.

nTemp: Optional[int] = None[source]#

None or an Int specifying the number of temperature points to be input. This argument is valid only when temperature = POINTWISE. The default value is None.

nodalThicknessField: str = ''[source]#

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements at each node. The nodalThicknessField argument applies only when thicknessType = NODAL_ANALYTICAL_FIELD or thicknessType = NODAL_DISCRETE_FIELD. The default value is an empty string.

poisson: float = 0[source]#

A Float specifying the Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

poissonDefinition: Literal[DEFAULT, VALUE] = DEFAULT[source]#

A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are: DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis. VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

preIntegrate: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether the shell section properties are specified by the user prior to the analysis (ON) or integrated during the analysis (OFF). The default value is OFF.

rebarLayers: Optional[RebarLayers] = None[source]#

A RebarLayers object specifying reinforcement properties.

setValues(symmetric=OFF, thicknessType=abaqusConstants.UNIFORM, preIntegrate=OFF, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, integrationRule=abaqusConstants.SIMPSON, temperature=abaqusConstants.GRADIENT, idealization=abaqusConstants.NO_IDEALIZATION, nTemp=None, thicknessModulus=None, useDensity=OFF, density=0, layupName='', thicknessField='', nodalThicknessField='')[source]#

This method modifies the CompositeShellSection object.

Note

Check CompositeShellSection.setValues on help.3ds.com/0.1..

Parameters:

  • symmetric (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.

  • thicknessType (Literal[UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, NODAL_DISCRETE_FIELD], default: UNIFORM) – A SymbolicConstant specifying the distribution used for defining the thickness of the elements. Possible values are UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, and NODAL_DISCRETE_FIELD. The default value is UNIFORM.

  • preIntegrate (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the shell section properties are specified by the user prior to the analysis (ON) or integrated during the analysis (OFF). The default value is OFF.

  • poissonDefinition (Literal[DEFAULT, VALUE], default: DEFAULT) – A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

  • poisson (float, default: 0) – A Float specifying the Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

  • integrationRule (Literal[SIMPSON, GAUSS], default: SIMPSON) – A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.

  • temperature (Literal[GRADIENT, POINTWISE], default: GRADIENT) – A SymbolicConstant specifying the mode used for temperature and field variable input across the section thickness. Possible values are GRADIENT and POINTWISE. The default value is GRADIENT.

  • idealization (Literal[NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, BENDING], default: NO_IDEALIZATION) – A SymbolicConstant specifying the mechanical idealization used for the section calculations. This member is only applicable when preIntegrate is set to ON. Possible values are NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, and BENDING. The default value is NO_IDEALIZATION.

  • nTemp (Optional[int], default: None) – None or an Int specifying the number of temperature points to be input. This argument is valid only when temperature = POINTWISE. The default value is None.

  • thicknessModulus (Optional[float], default: None) – None or a Float specifying the effective thickness modulus. This argument is relevant only for continuum shells and must be used in conjunction with the argument poisson. The default value is None.

  • useDensity (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not to use the value of density. The default value is OFF.

  • density (float, default: 0) – A Float specifying the value of density to apply to this section. The default value is 0.0.

  • layupName (str, default: '') – A String specifying the layup name for this section. The default value is an empty string.

  • thicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements. The thicknessField argument applies only when thicknessType = ANALYTICAL_FIELD or thicknessType = DISCRETE_FIELD. The default value is an empty string.

  • nodalThicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements at each node. The nodalThicknessField argument applies only when thicknessType = NODAL_ANALYTICAL_FIELD or thicknessType = NODAL_DISCRETE_FIELD. The default value is an empty string.

symmetric: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.

temperature: Literal[GRADIENT, POINTWISE] = GRADIENT[source]#

A SymbolicConstant specifying the mode used for temperature and field variable input across the section thickness. Possible values are GRADIENT and POINTWISE. The default value is GRADIENT.

thicknessField: str = ''[source]#

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements. The thicknessField argument applies only when thicknessType = ANALYTICAL_FIELD or thicknessType = DISCRETE_FIELD. The default value is an empty string.

thicknessModulus: Optional[float] = None[source]#

None or a Float specifying the effective thickness modulus. This argument is relevant only for continuum shells and must be used in conjunction with the argument poisson. The default value is None.

thicknessType: Literal[UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, NODAL_DISCRETE_FIELD] = UNIFORM[source]#

A SymbolicConstant specifying the distribution used for defining the thickness of the elements. Possible values are UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, and NODAL_DISCRETE_FIELD. The default value is UNIFORM.

transverseShear: Optional[TransverseShearShell] = None[source]#

A TransverseShearShell object specifying the transverse shear stiffness properties.

useDensity: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether or not to use the value of density. The default value is OFF.

CompositeSolidSection#

class CompositeSolidSection(name, layup, symmetric=OFF, layupName='')[source]#

The CompositeSolidSection object defines the properties of a composite solid section. The CompositeSolidSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • SOLID SECTION

Note

Check CompositeSolidSection on help.3ds.com/0.1..

Public Data Attributes:

symmetric

A Boolean specifying whether or not the layup should be made symmetric by the analysis.

layupName

A String specifying the layup name for this section.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

__init__(name, layup[, symmetric, layupName])

This method creates a CompositeSolidSection object.

setValues([symmetric, layupName])

This method modifies the CompositeSolidSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
layup: List[SectionLayer][source]#

A SectionLayerArray object specifying the solid cross-section.

layupName: str = ''[source]#

A String specifying the layup name for this section. The default value is an empty string.

setValues(symmetric=OFF, layupName='')[source]#

This method modifies the CompositeSolidSection object.

Note

Check CompositeSolidSection.setValues on help.3ds.com/0.1..

Parameters:

  • symmetric (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.

  • layupName (str, default: '') – A String specifying the layup name for this section. The default value is an empty string.

symmetric: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.

ConnectorSection#

class ConnectorSection(name, assembledType=abaqusConstants.NONE, rotationalType=abaqusConstants.NONE, translationalType=abaqusConstants.NONE, integration=abaqusConstants.UNSPECIFIED, u1ReferenceLength=None, u2ReferenceLength=None, u3ReferenceLength=None, ur1ReferenceAngle=None, ur2ReferenceAngle=None, ur3ReferenceAngle=None, massPerLength=None, contactAngle=None, materialFlowFactor=1, regularize=ON, defaultTolerance=ON, regularization=0, extrapolation=abaqusConstants.CONSTANT, behaviorOptions=Ellipsis)[source]#

A ConnectorSection object describes the connection type and the behavior of a connector. The ConnectorSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • CONNECTOR SECTION

  • CONNECTOR BEHAVIOR

  • CONNECTOR CONSTITUTIVE REFERENCE

Note

Check ConnectorSection on help.3ds.com/0.1..

Public Data Attributes:

assembledType

A SymbolicConstant specifying the assembled connection type.

rotationalType

default value is NONE.You cannot include the rotationalType argument if assembledType is given a value other than NONE.

translationalType

A SymbolicConstant specifying the basic translational connection type.

integration

A SymbolicConstant specifying the time integration scheme to use for analysis.

u1ReferenceLength

None or a Float specifying the reference length associated with constitutive response for the first component of relative motion.

u2ReferenceLength

None or a Float specifying the reference length associated with constitutive response for the second component of relative motion.

u3ReferenceLength

None or a Float specifying the reference length associated with constitutive response for the third component of relative motion.

ur1ReferenceAngle

None or a Float specifying the reference angle in degrees associated with constitutive response for the fourth component of relative motion.

ur2ReferenceAngle

None or a Float specifying the reference angle in degrees associated with constitutive response for the fifth component of relative motion.

ur3ReferenceAngle

None or a Float specifying the reference angle in degrees associated with constitutive response for the sixth component of relative motion.

massPerLength

None or a Float specifying the mass per unit reference length of belt material.

contactAngle

None or a Float specifying the contact angle made by the belt wrapping around node b.

materialFlowFactor

A Float specifying the scaling factor for material flow at node b.

regularize

A Boolean specifying whether or not all tabular data associated with the behaviorOptions will be regularized.

defaultTolerance

A Boolean specifying whether or not the default regularization tolerance will be used for all tabular data associated with the behaviorOptions.

regularization

A Float specifying the regularization increment to be used for all tabular data associated with the behaviorOptions.

extrapolation

A SymbolicConstant specifying the extrapolation technique to be used for all tabular data associated with the behaviorOptions.

behaviorOptions

A ConnectorBehaviorOptionArray object.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

__init__(name[, assembledType, ...])

This method creates a ConnectorSection object.

setValues([assembledType, rotationalType, ...])

This method modifies the ConnectorSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
assembledType: Literal[NONE, BEAM, BUSHING, CVJOINT, CYLINDRICAL, HINGE, PLANAR, RETRACTOR, SLIPRING, TRANSLATOR, UJOINT, WELD] = NONE[source]#

A SymbolicConstant specifying the assembled connection type. Possible values are: NONE, BEAM, BUSHING, CVJOINT, CYLINDRICAL, HINGE, PLANAR, RETRACTOR, SLIPRING, TRANSLATOR, UJOINT, WELD The default value is NONE.You cannot include the assembledType argument if translationalType or rotationalType are given a value other than NONE. At least one of the arguments assembledType, translationalType, or rotationalType must be given a value other than NONE.

behaviorOptions: Optional[List[ConnectorBehaviorOption]] = None[source]#

A ConnectorBehaviorOptionArray object.

contactAngle: Optional[float] = None[source]#

None or a Float specifying the contact angle made by the belt wrapping around node b. This argument is applicable only to an Abaqus/Explicit analysis, and only when assembledType = SLIPRING. The default value is None.

defaultTolerance: Union[AbaqusBoolean, bool] = ON[source]#

A Boolean specifying whether or not the default regularization tolerance will be used for all tabular data associated with the behaviorOptions. This argument is applicable only for an Abaqus/Explicit analysis and only if regularize = ON. The default value is ON.

extrapolation: Literal[CONSTANT, LINEAR] = CONSTANT[source]#

A SymbolicConstant specifying the extrapolation technique to be used for all tabular data associated with the behaviorOptions. Possible values are CONSTANT and LINEAR. The default value is CONSTANT.

integration: Literal[UNSPECIFIED, IMPLICIT, EXPLICIT] = UNSPECIFIED[source]#

A SymbolicConstant specifying the time integration scheme to use for analysis. This argument is applicable only to an Abaqus/Explicit analysis. Possible values are UNSPECIFIED, IMPLICIT, and EXPLICIT. The default value is UNSPECIFIED.

massPerLength: Optional[float] = None[source]#

None or a Float specifying the mass per unit reference length of belt material. This argument is applicable only when assembledType = SLIPRING, and must be specified in that case. The default value is None.

materialFlowFactor: float = 1[source]#

A Float specifying the scaling factor for material flow at node b. This argument is applicable only when assembledType = RETRACTOR or rotationalType = FLOW_CONVERTER. The default value is 1.0.

regularization: float = 0[source]#

A Float specifying the regularization increment to be used for all tabular data associated with the behaviorOptions. This argument is applicable only for an Abaqus/Explicit analysis and only if regularize = ON and defaultTolerance = OFF. The default value is 0.03.

regularize: Union[AbaqusBoolean, bool] = ON[source]#

A Boolean specifying whether or not all tabular data associated with the behaviorOptions will be regularized. This argument is applicable only for an Abaqus/Explicit analysis. The default value is ON.

rotationalType: Literal[NONE, ALIGN, CARDAN, CONSTANT_VELOCITY, EULER, FLEXION_TORSION, FLOW_CONVERTER, PROJECTION_FLEXION_TORSION, REVOLUTE, ROTATION, ROTATION_ACCELEROMETER, UNIVERSAL] = NONE[source]#

default value is NONE.You cannot include the rotationalType argument if assembledType is given a value other than NONE. At least one of the arguments assembledType, translationalType, or rotationalType must be given an value other than NONE.

setValues(assembledType=abaqusConstants.NONE, rotationalType=abaqusConstants.NONE, translationalType=abaqusConstants.NONE, integration=abaqusConstants.UNSPECIFIED, u1ReferenceLength=None, u2ReferenceLength=None, u3ReferenceLength=None, ur1ReferenceAngle=None, ur2ReferenceAngle=None, ur3ReferenceAngle=None, massPerLength=None, contactAngle=None, materialFlowFactor=1, regularize=ON, defaultTolerance=ON, regularization=0, extrapolation=abaqusConstants.CONSTANT, behaviorOptions=Ellipsis)[source]#

This method modifies the ConnectorSection object.

Note

Check ConnectorSection.setValues on help.3ds.com/0.1..

Parameters:

  • assembledType (Literal[NONE, BEAM, BUSHING, CVJOINT, CYLINDRICAL, HINGE, PLANAR, RETRACTOR, SLIPRING, TRANSLATOR, UJOINT, WELD], default: NONE) – A SymbolicConstant specifying the assembled connection type. Possible values are:NONEBEAMBUSHINGCVJOINTCYLINDRICALHINGEPLANARRETRACTORSLIPRINGTRANSLATORUJOINTWELDThe default value is NONE.You cannot include the assembledType argument if translationalType or rotationalType are given a value other than NONE. At least one of the arguments assembledType, translationalType, or rotationalType must be given a value other than NONE.

  • rotationalType (Literal[NONE, ALIGN, CARDAN, CONSTANT_VELOCITY, EULER, FLEXION_TORSION, FLOW_CONVERTER, PROJECTION_FLEXION_TORSION, REVOLUTE, ROTATION, ROTATION_ACCELEROMETER, UNIVERSAL], default: NONE) – A SymbolicConstant specifying the basic rotational connection type. Possible values are:NONEALIGNCARDANCONSTANT_VELOCITYEULERFLEXION_TORSIONFLOW_CONVERTERPROJECTION_FLEXION_TORSIONREVOLUTEROTATIONROTATION_ACCELEROMETERUNIVERSALThe default value is NONE.You cannot include the rotationalType argument if assembledType is given a value other than NONE. At least one of the arguments assembledType, translationalType, or rotationalType must be given an value other than NONE.

  • translationalType (Literal[NONE, ACCELEROMETER, AXIAL, CARTESIAN, JOIN, LINK, PROJECTION_CARTESIAN, RADIAL_THRUST, SLIDE_PLANE, SLOT], default: NONE) – A SymbolicConstant specifying the basic translational connection type. Possible values are:NONEACCELEROMETERAXIALCARTESIANJOINLINKPROJECTION_CARTESIANRADIAL_THRUSTSLIDE_PLANESLOTThe default value is NONE.You cannot include the translationalType argument if assembledType is given a value other than NONE. At least one of the arguments assembledType, translationalType, or rotationalType must be given an value other than NONE.

  • integration (Literal[UNSPECIFIED, IMPLICIT, EXPLICIT], default: UNSPECIFIED) – A SymbolicConstant specifying the time integration scheme to use for analysis. This argument is applicable only to an Abaqus/Explicit analysis. Possible values are UNSPECIFIED, IMPLICIT, and EXPLICIT. The default value is UNSPECIFIED.

  • u1ReferenceLength (Optional[float], default: None) – None or a Float specifying the reference length associated with constitutive response for the first component of relative motion. The default value is None.

  • u2ReferenceLength (Optional[float], default: None) – None or a Float specifying the reference length associated with constitutive response for the second component of relative motion. The default value is None.

  • u3ReferenceLength (Optional[float], default: None) – None or a Float specifying the reference length associated with constitutive response for the third component of relative motion. The default value is None.

  • ur1ReferenceAngle (Optional[float], default: None) – None or a Float specifying the reference angle in degrees associated with constitutive response for the fourth component of relative motion. The default value is None.

  • ur2ReferenceAngle (Optional[float], default: None) – None or a Float specifying the reference angle in degrees associated with constitutive response for the fifth component of relative motion. The default value is None.

  • ur3ReferenceAngle (Optional[float], default: None) – None or a Float specifying the reference angle in degrees associated with constitutive response for the sixth component of relative motion. The default value is None.

  • massPerLength (Optional[float], default: None) – None or a Float specifying the mass per unit reference length of belt material. This argument is applicable only when assembledType = SLIPRING, and must be specified in that case. The default value is None.

  • contactAngle (Optional[float], default: None) – None or a Float specifying the contact angle made by the belt wrapping around node b. This argument is applicable only to an Abaqus/Explicit analysis, and only when assembledType = SLIPRING. The default value is None.

  • materialFlowFactor (float, default: 1) – A Float specifying the scaling factor for material flow at node b. This argument is applicable only when assembledType = RETRACTOR or rotationalType = FLOW_CONVERTER. The default value is 1.0.

  • regularize (Union[AbaqusBoolean, bool], default: ON) – A Boolean specifying whether or not all tabular data associated with the behaviorOptions will be regularized. This argument is applicable only for an Abaqus/Explicit analysis. The default value is ON.

  • defaultTolerance (Union[AbaqusBoolean, bool], default: ON) – A Boolean specifying whether or not the default regularization tolerance will be used for all tabular data associated with the behaviorOptions. This argument is applicable only for an Abaqus/Explicit analysis and only if regularize = ON. The default value is ON.

  • regularization (float, default: 0) – A Float specifying the regularization increment to be used for all tabular data associated with the behaviorOptions. This argument is applicable only for an Abaqus/Explicit analysis and only if regularize = ON and defaultTolerance = OFF. The default value is 0.03.

  • extrapolation (Literal[CONSTANT, LINEAR], default: CONSTANT) – A SymbolicConstant specifying the extrapolation technique to be used for all tabular data associated with the behaviorOptions. Possible values are CONSTANT and LINEAR. The default value is CONSTANT.

  • behaviorOptions (List[ConnectorBehaviorOption], default: Ellipsis) – A ConnectorBehaviorOptionArray object.

Raises:

RangeError –

translationalType: Literal[NONE, ACCELEROMETER, AXIAL, CARTESIAN, JOIN, LINK, PROJECTION_CARTESIAN, RADIAL_THRUST, SLIDE_PLANE, SLOT] = NONE[source]#

A SymbolicConstant specifying the basic translational connection type. Possible values are: NONE, ACCELEROMETER, AXIAL, CARTESIAN, JOIN, LINK, PROJECTION_CARTESIAN, RADIAL_THRUST, SLIDE_PLANE, SLOT Thedefault value is NONE. You cannot include the translationalType argument if assembledType is given a value other than NONE. At least one of the arguments assembledType, translationalType, or rotationalType must be given an value other than NONE.

u1ReferenceLength: Optional[float] = None[source]#

None or a Float specifying the reference length associated with constitutive response for the first component of relative motion. The default value is None.

u2ReferenceLength: Optional[float] = None[source]#

None or a Float specifying the reference length associated with constitutive response for the second component of relative motion. The default value is None.

u3ReferenceLength: Optional[float] = None[source]#

None or a Float specifying the reference length associated with constitutive response for the third component of relative motion. The default value is None.

ur1ReferenceAngle: Optional[float] = None[source]#

None or a Float specifying the reference angle in degrees associated with constitutive response for the fourth component of relative motion. The default value is None.

ur2ReferenceAngle: Optional[float] = None[source]#

None or a Float specifying the reference angle in degrees associated with constitutive response for the fifth component of relative motion. The default value is None.

ur3ReferenceAngle: Optional[float] = None[source]#

None or a Float specifying the reference angle in degrees associated with constitutive response for the sixth component of relative motion. The default value is None.

EulerianSection#

class EulerianSection(name, data)[source]#

The EulerianSection object defines the properties of a Eulerian section. The EulerianSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • EULERIAN SECTION

Note

Check EulerianSection on help.3ds.com/0.1..

Public Data Attributes:

Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

__init__(name, data)

This method creates a EulerianSection object.

setValues(*args, **kwargs)

This method modifies the EulerianSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
data: str[source]#

A String-to-String Dictionary specifying a dictionary mapping Material instance names to Material names. Internally the specified mapping gets sorted on Material instance name.

setValues(*args, **kwargs)[source]#

This method modifies the EulerianSection object.

GasketSection#

class GasketSection(name, material, crossSection=1, initialGap=0, initialThickness=abaqusConstants.DEFAULT, initialVoid=0, stabilizationStiffness=abaqusConstants.DEFAULT)[source]#

The GasketSection object defines the properties of a gasket section. The GasketSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • GASKET SECTION

Note

Check GasketSection on help.3ds.com/0.1..

Public Data Attributes:

crossSection

A Float specifying the cross-sectional area, width, or out-of-plane thickness, if applicable, depending on the gasket element type.

initialGap

A Float specifying the initial gap.

initialThickness

The SymbolicConstant DEFAULT or a Float specifying the initial gasket thickness.

initialVoid

A Float specifying the initial void.

stabilizationStiffness

The SymbolicConstant DEFAULT or a Float specifying the default stabilization stiffness used in all but link elements to stabilize gasket elements that are not supported at all nodes, such as those that extend outside neighboring components.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

__init__(name, material[, crossSection, ...])

This method creates a GasketSection object.

setValues([crossSection, initialGap, ...])

This method modifies the GasketSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
crossSection: float = 1[source]#

A Float specifying the cross-sectional area, width, or out-of-plane thickness, if applicable, depending on the gasket element type. The default value is 1.0.

initialGap: float = 0[source]#

A Float specifying the initial gap. The default value is 0.0.

initialThickness: Union[SymbolicConstant, float] = DEFAULT[source]#

The SymbolicConstant DEFAULT or a Float specifying the initial gasket thickness. If DEFAULT is specified, the initial thickness is determined using nodal coordinates. The default value is DEFAULT.

initialVoid: float = 0[source]#

A Float specifying the initial void. The default value is 0.0.

material: str[source]#

A String specifying the name of the material of which the gasket is made or material that defines gasket behavior.

setValues(crossSection=1, initialGap=0, initialThickness=abaqusConstants.DEFAULT, initialVoid=0, stabilizationStiffness=abaqusConstants.DEFAULT)[source]#

This method modifies the GasketSection object.

Note

Check GasketSection.setValues on help.3ds.com/0.1..

Parameters:

  • crossSection (float, default: 1) – A Float specifying the cross-sectional area, width, or out-of-plane thickness, if applicable, depending on the gasket element type. The default value is 1.0.

  • initialGap (float, default: 0) – A Float specifying the initial gap. The default value is 0.0.

  • initialThickness (Union[SymbolicConstant, float], default: DEFAULT) – The SymbolicConstant DEFAULT or a Float specifying the initial gasket thickness. If DEFAULT is specified, the initial thickness is determined using nodal coordinates. The default value is DEFAULT.

  • initialVoid (float, default: 0) – A Float specifying the initial void. The default value is 0.0.

  • stabilizationStiffness (Union[SymbolicConstant, float], default: DEFAULT) – The SymbolicConstant DEFAULT or a Float specifying the default stabilization stiffness used in all but link elements to stabilize gasket elements that are not supported at all nodes, such as those that extend outside neighboring components. If DEFAULT is specified, a value is used equal to 10-9 times the initial compressive stiffness in the thickness direction. The default value is DEFAULT.

Raises:

ValueError –

stabilizationStiffness: Union[SymbolicConstant, float] = DEFAULT[source]#

The SymbolicConstant DEFAULT or a Float specifying the default stabilization stiffness used in all but link elements to stabilize gasket elements that are not supported at all nodes, such as those that extend outside neighboring components. If DEFAULT is specified, a value is used equal to 10-9 times the initial compressive stiffness in the thickness direction. The default value is DEFAULT.

GeneralStiffnessSection#

class GeneralStiffnessSection(name, stiffnessMatrix, referenceTemperature=None, applyThermalStress=OFF, temperatureDependency=OFF, dependencies=0, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, useDensity=OFF, density=0, thermalStresses=(), scalingData=())[source]#

The GeneralStiffnessSection object defines the properties of a shell section via the stiffness matrix. The GeneralStiffnessSection object is derived from the ShellSection object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • SHELL GENERAL SECTION

Note

Check GeneralStiffnessSection on help.3ds.com/0.1..

Public Data Attributes:

rebarLayers

A RebarLayers object specifying reinforcement properties.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.

referenceTemperature

None or a Float specifying the reference temperature for thermal expansion.

applyThermalStress

A Boolean specifying whether or not the section stiffness varies with thermal stresses.

temperatureDependency

A Boolean specifying whether the data depend on temperature.

dependencies

An Int specifying the number of field variable dependencies.

poissonDefinition

A SymbolicConstant specifying whether to use the default value for the Poisson's ratio.

poisson

A Float specifying the Poisson's ratio.

useDensity

A Boolean specifying whether or not to use the value of density.

density

A Float specifying the value of density to apply to this section.

thermalStresses

A sequence of Floats specifying the generalized stress values caused by a unit temperature rise.

scalingData

A sequence of sequences of Floats specifying the scaling factors for given temperatures and/or field data.
Inherited from ShellSection

name

A String specifying the repository key.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.

Public Methods:

__init__(name, stiffnessMatrix[, ...])

This method creates a GeneralStiffnessSection object.

setValues([referenceTemperature, ...])

This method modifies the GeneralStiffnessSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
applyThermalStress: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether or not the section stiffness varies with thermal stresses. The default value is OFF.

density: float = 0[source]#

A Float specifying the value of density to apply to this section. The default value is 0.0.

dependencies: int = 0[source]#

An Int specifying the number of field variable dependencies. The default value is 0.

poisson: float = 0[source]#

A Float specifying the Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

poissonDefinition: Literal[VALUE, DEFAULT] = DEFAULT[source]#

A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

rebarLayers: Optional[RebarLayers] = None[source]#

A RebarLayers object specifying reinforcement properties.

referenceTemperature: Optional[float] = None[source]#

None or a Float specifying the reference temperature for thermal expansion. The default value is None.

scalingData: tuple = ()[source]#

A sequence of sequences of Floats specifying the scaling factors for given temperatures and/or field data. Each row should contain (Y, alpha, T, F1,…,Fn). The default value is an empty sequence.

setValues(referenceTemperature=None, applyThermalStress=OFF, temperatureDependency=OFF, dependencies=0, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, useDensity=OFF, density=0, thermalStresses=(), scalingData=())[source]#

This method modifies the GeneralStiffnessSection object.

Note

Check GeneralStiffnessSection.setValues on help.3ds.com/0.1..

Parameters:

  • referenceTemperature (Optional[float], default: None) – None or a Float specifying the reference temperature for thermal expansion. The default value is None.

  • applyThermalStress (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not the section stiffness varies with thermal stresses. The default value is OFF.

  • temperatureDependency (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the data depend on temperature. The default value is OFF.

  • dependencies (int, default: 0) – An Int specifying the number of field variable dependencies. The default value is 0.

  • poissonDefinition (Literal[VALUE, DEFAULT], default: DEFAULT) – A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

  • poisson (float, default: 0) – A Float specifying the Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

  • useDensity (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not to use the value of density. The default value is OFF.

  • density (float, default: 0) – A Float specifying the value of density to apply to this section. The default value is 0.0.

  • thermalStresses (tuple, default: ()) – A sequence of Floats specifying the generalized stress values caused by a unit temperature rise. Six entries must be given if the value of applyThermalStress is set to True. The default value is (“”).

  • scalingData (tuple, default: ()) – A sequence of sequences of Floats specifying the scaling factors for given temperatures and/or field data. Each row should contain (Y, alpha, T, F1,…,Fn). The default value is an empty sequence.

stiffnessMatrix: tuple[source]#

A sequence of Floats specifying the stiffness matrix for the section in the order D11, D12, D22, D13, D23, D33, …., D66. Twenty-one entries must be given.

temperatureDependency: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether the data depend on temperature. The default value is OFF.

thermalStresses: tuple = ()[source]#

A sequence of Floats specifying the generalized stress values caused by a unit temperature rise. Six entries must be given if the value of applyThermalStress is set to True. The default value is (“”).

transverseShear: Optional[TransverseShearShell] = None[source]#

A TransverseShearShell object specifying the transverse shear stiffness properties.

useDensity: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether or not to use the value of density. The default value is OFF.

GeometryShellSection#

class GeometryShellSection(nodalThicknessField='', thicknessField='', thicknessType=abaqusConstants.UNIFORM, preIntegrate=OFF, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, integrationRule=abaqusConstants.SIMPSON, temperature=abaqusConstants.GRADIENT, nTemp=None, thicknessModulus=None, useDensity=OFF, density=0)[source]#

The GeometryShellSection object defines the properties of a geometry shell section. The GeometryShellSection object has no explicit constructor and no methods. The GeometryShellSection object is an abstract base type. The GeometryShellSection object is derived from the ShellSection object.

Note

This object can be accessed by:

import section
mdb.models[name].parts[name].compositeLayups[i].section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

Note

Check GeometryShellSection on help.3ds.com/0.1..

Public Data Attributes:

name

A String specifying the repository key.

thicknessType

A SymbolicConstant specifying the distribution used for defining the thickness of the elements.

preIntegrate

A Boolean specifying whether the shell section properties are specified by the user prior to the analysis (ON) or integrated during the analysis (OFF).

poissonDefinition

A SymbolicConstant specifying whether to use the default value for the Poisson's ratio.

poisson

A Float specifying the Poisson's ratio.

integrationRule

A SymbolicConstant specifying the shell section integration rule.

temperature

A SymbolicConstant specifying the mode used for temperature and field variable input across the section thickness.

idealization

A SymbolicConstant specifying the mechanical idealization used for the section calculations.

nTemp

None or an Int specifying the number of temperature points to be input.

thicknessModulus

None or a Float specifying the effective thickness modulus.

useDensity

A Boolean specifying whether or not to use the value of density.

density

A Float specifying the value of density to apply to this section.

thicknessField

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements.

rebarLayers

A RebarLayers object specifying reinforcement properties.

nodalThicknessField

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements at each node.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.
Inherited from ShellSection

name

A String specifying the repository key.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.

Public Methods:

__init__([nodalThicknessField, ...])

This method creates a GeometryShellSection object.

RebarLayers(rebarSpacing, layerTable)

This method creates a RebarLayers object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
RebarLayers(rebarSpacing, layerTable)[source]#

This method creates a RebarLayers object.

Note

This function can be accessed by:

mdb.models[name].parts[name].compositeLayups[name].Section

Note

Check RebarLayers on help.3ds.com/0.1..

Parameters:
Returns:

A RebarLayers object.

Return type:

RebarLayers

density: float = 0[source]#

A Float specifying the value of density to apply to this section. The default value is 0.0.

idealization: SymbolicConstant = NO_IDEALIZATION[source]#

A SymbolicConstant specifying the mechanical idealization used for the section calculations. This member is only applicable when preIntegrate is set to ON. Possible values are NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, and BENDING. The default value is NO_IDEALIZATION.

integrationRule: SymbolicConstant = SIMPSON[source]#

A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.

nTemp: Optional[int] = None[source]#

None or an Int specifying the number of temperature points to be input. This argument is valid only when temperature = POINTWISE. The default value is None.

name: str = ''[source]#

A String specifying the repository key.

nodalThicknessField: str = ''[source]#

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements at each node. The nodalThicknessField argument applies only when thicknessType = NODAL_ANALYTICAL_FIELD or thicknessType = NODAL_DISCRETE_FIELD. The default value is an empty string.

poisson: float = 0[source]#

A Float specifying the Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

poissonDefinition: SymbolicConstant = DEFAULT[source]#

A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

preIntegrate: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether the shell section properties are specified by the user prior to the analysis (ON) or integrated during the analysis (OFF). The default value is OFF.

rebarLayers: RebarLayers = <abaqus.Section.RebarLayers.RebarLayers object>[source]#

A RebarLayers object specifying reinforcement properties.

temperature: SymbolicConstant = GRADIENT[source]#

A SymbolicConstant specifying the mode used for temperature and field variable input across the section thickness. Possible values are GRADIENT and POINTWISE. The default value is GRADIENT.

thicknessField: str = ''[source]#

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements. The thicknessField argument applies only when thicknessType = ANALYTICAL_FIELD or thicknessType = DISCRETE_FIELD. The default value is an empty string.

thicknessModulus: Optional[float] = None[source]#

None or a Float specifying the effective thickness modulus. This argument is relevant only for continuum shells and must be used in conjunction with the argument poisson. The default value is None.

thicknessType: SymbolicConstant = UNIFORM[source]#

A SymbolicConstant specifying the distribution used for defining the thickness of the elements. Possible values are UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, and NODAL_DISCRETE_FIELD. The default value is UNIFORM.

transverseShear: Optional[TransverseShearShell] = None[source]#

A TransverseShearShell object specifying the transverse shear stiffness properties.

useDensity: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether or not to use the value of density. The default value is OFF.

HomogeneousShellSection#

class HomogeneousShellSection(name, material, thickness=0, numIntPts=5, thicknessType=abaqusConstants.UNIFORM, preIntegrate=OFF, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, integrationRule=abaqusConstants.SIMPSON, temperature=abaqusConstants.GRADIENT, idealization=abaqusConstants.NO_IDEALIZATION, nTemp=None, thicknessModulus=None, useDensity=OFF, density=0, thicknessField='', nodalThicknessField='')[source]#

The HomogeneousShellSection object defines the properties of a shell section. The HomogeneousShellSection object is derived from the GeometryShellSection object.

Note

This object can be accessed by:

import section
mdb.models[name].parts[name].compositeLayups[i].section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • SHELL SECTION

  • SHELL GENERAL SECTION

Note

Check HomogeneousShellSection on help.3ds.com/0.1..

Public Data Attributes:

rebarLayers

A RebarLayers object specifying reinforcement properties.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.

thickness

A Float specifying the thickness of the section.

numIntPts

An Int specifying the number of integration points to be used through the section.

thicknessType

A SymbolicConstant specifying the distribution used for defining the thickness of the elements.

preIntegrate

A Boolean specifying whether the shell section properties are specified by the user prior to the analysis (ON) or integrated during the analysis (OFF).

poissonDefinition

A SymbolicConstant specifying whether to use the default value for the Poisson's ratio.

poisson

A Float specifying the Poisson's ratio.

integrationRule

A SymbolicConstant specifying the shell section integration rule.

temperature

A SymbolicConstant specifying the mode used for temperature and field variable input across the section thickness.

idealization

A SymbolicConstant specifying the mechanical idealization used for the section calculations.

nTemp

None or an Int specifying the number of temperature points to be input.

thicknessModulus

None or a Float specifying the effective thickness modulus.

useDensity

A Boolean specifying whether or not to use the value of density.

density

A Float specifying the value of density to apply to this section.

thicknessField

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements.

nodalThicknessField

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements at each node.
Inherited from GeometryShellSection

name

A String specifying the repository key.

thicknessType

A SymbolicConstant specifying the distribution used for defining the thickness of the elements.

preIntegrate

A Boolean specifying whether the shell section properties are specified by the user prior to the analysis (ON) or integrated during the analysis (OFF).

poissonDefinition

A SymbolicConstant specifying whether to use the default value for the Poisson's ratio.

poisson

A Float specifying the Poisson's ratio.

integrationRule

A SymbolicConstant specifying the shell section integration rule.

temperature

A SymbolicConstant specifying the mode used for temperature and field variable input across the section thickness.

idealization

A SymbolicConstant specifying the mechanical idealization used for the section calculations.

nTemp

None or an Int specifying the number of temperature points to be input.

thicknessModulus

None or a Float specifying the effective thickness modulus.

useDensity

A Boolean specifying whether or not to use the value of density.

density

A Float specifying the value of density to apply to this section.

thicknessField

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements.

rebarLayers

A RebarLayers object specifying reinforcement properties.

nodalThicknessField

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements at each node.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.
Inherited from ShellSection

name

A String specifying the repository key.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.

Public Methods:

__init__(name, material[, thickness, ...])

This method creates a HomogeneousShellSection object.

setValues([thickness, numIntPts, ...])

This method modifies the HomogeneousShellSection object.
Inherited from GeometryShellSection

__init__(name, material[, thickness, ...])

This method creates a HomogeneousShellSection object.

RebarLayers(rebarSpacing, layerTable)

This method creates a RebarLayers object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
density: float = 0[source]#

A Float specifying the value of density to apply to this section. The default value is 0.0.

idealization: Literal[NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, BENDING] = NO_IDEALIZATION[source]#

A SymbolicConstant specifying the mechanical idealization used for the section calculations. This member is only applicable when preIntegrate is set to ON. Possible values are NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, and BENDING. The default value is NO_IDEALIZATION.

integrationRule: Literal[SIMPSON, GAUSS] = SIMPSON[source]#

A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.

material: str[source]#

A String specifying the name of the section material.

nTemp: Optional[int] = None[source]#

None or an Int specifying the number of temperature points to be input. This argument is valid only when temperature = POINTWISE. The default value is None.

nodalThicknessField: str = ''[source]#

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements at each node. The nodalThicknessField argument applies only when thicknessType = NODAL_ANALYTICAL_FIELD or thicknessType = NODAL_DISCRETE_FIELD. The default value is an empty string.

numIntPts: int = 5[source]#

An Int specifying the number of integration points to be used through the section. Possible values are numIntPts >> 0. The default value is 5.To use the default settings of the analysis products, set numIntPts to 5 if integrationRule = SIMPSON or set numIntPts to 7 if integrationRule = GAUSS.

poisson: float = 0[source]#

A Float specifying the Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

poissonDefinition: Literal[VALUE, DEFAULT] = DEFAULT[source]#

A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

preIntegrate: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether the shell section properties are specified by the user prior to the analysis (ON) or integrated during the analysis (OFF). The default value is OFF.

rebarLayers: Optional[RebarLayers] = None[source]#

A RebarLayers object specifying reinforcement properties.

setValues(thickness=0, numIntPts=5, thicknessType=abaqusConstants.UNIFORM, preIntegrate=OFF, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, integrationRule=abaqusConstants.SIMPSON, temperature=abaqusConstants.GRADIENT, idealization=abaqusConstants.NO_IDEALIZATION, nTemp=None, thicknessModulus=None, useDensity=OFF, density=0, thicknessField='', nodalThicknessField='')[source]#

This method modifies the HomogeneousShellSection object.

Note

Check HomogeneousShellSection.setValues on help.3ds.com/0.1..

Parameters:

  • thickness (float, default: 0) – A Float specifying the thickness of the section. The thickness argument applies only when thicknessType = UNIFORM. The default value is 0.0.

  • numIntPts (int, default: 5) – An Int specifying the number of integration points to be used through the section. Possible values are numIntPts >> 0. The default value is 5.To use the default settings of the analysis products, set numIntPts to 5 if integrationRule = SIMPSON or set numIntPts to 7 if integrationRule = GAUSS.

  • thicknessType (Literal[UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, NODAL_DISCRETE_FIELD], default: UNIFORM) – A SymbolicConstant specifying the distribution used for defining the thickness of the elements. Possible values are UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, and NODAL_DISCRETE_FIELD. The default value is UNIFORM.

  • preIntegrate (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the shell section properties are specified by the user prior to the analysis (ON) or integrated during the analysis (OFF). The default value is OFF.

  • poissonDefinition (Literal[VALUE, DEFAULT], default: DEFAULT) – A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

  • poisson (float, default: 0) – A Float specifying the Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

  • integrationRule (Literal[SIMPSON, GAUSS], default: SIMPSON) – A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.

  • temperature (Literal[GRADIENT, POINTWISE], default: GRADIENT) – A SymbolicConstant specifying the mode used for temperature and field variable input across the section thickness. Possible values are GRADIENT and POINTWISE. The default value is GRADIENT.

  • idealization (Literal[NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, BENDING], default: NO_IDEALIZATION) – A SymbolicConstant specifying the mechanical idealization used for the section calculations. This member is only applicable when preIntegrate is set to ON. Possible values are NO_IDEALIZATION, SMEAR_ALL_LAYERS, MEMBRANE, and BENDING. The default value is NO_IDEALIZATION.

  • nTemp (Optional[int], default: None) – None or an Int specifying the number of temperature points to be input. This argument is valid only when temperature = POINTWISE. The default value is None.

  • thicknessModulus (Optional[float], default: None) – None or a Float specifying the effective thickness modulus. This argument is relevant only for continuum shells and must be used in conjunction with the argument poisson. The default value is None.

  • useDensity (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether or not to use the value of density. The default value is OFF.

  • density (float, default: 0) – A Float specifying the value of density to apply to this section. The default value is 0.0.

  • thicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements. The thicknessField argument applies only when thicknessType = ANALYTICAL_FIELD or thicknessType = DISCRETE_FIELD. The default value is an empty string.

  • nodalThicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements at each node. The nodalThicknessField argument applies only when thicknessType = NODAL_ANALYTICAL_FIELD or thicknessType = NODAL_DISCRETE_FIELD. The default value is an empty string.

temperature: Literal[GRADIENT, POINTWISE] = GRADIENT[source]#

A SymbolicConstant specifying the mode used for temperature and field variable input across the section thickness. Possible values are GRADIENT and POINTWISE. The default value is GRADIENT.

thickness: float = 0[source]#

A Float specifying the thickness of the section. The thickness argument applies only when thicknessType = UNIFORM. The default value is 0.0.

thicknessField: str = ''[source]#

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements. The thicknessField argument applies only when thicknessType = ANALYTICAL_FIELD or thicknessType = DISCRETE_FIELD. The default value is an empty string.

thicknessModulus: Optional[float] = None[source]#

None or a Float specifying the effective thickness modulus. This argument is relevant only for continuum shells and must be used in conjunction with the argument poisson. The default value is None.

thicknessType: Literal[UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, NODAL_DISCRETE_FIELD] = UNIFORM[source]#

A SymbolicConstant specifying the distribution used for defining the thickness of the elements. Possible values are UNIFORM, ANALYTICAL_FIELD, DISCRETE_FIELD, NODAL_ANALYTICAL_FIELD, and NODAL_DISCRETE_FIELD. The default value is UNIFORM.

transverseShear: Optional[TransverseShearShell] = None[source]#

A TransverseShearShell object specifying the transverse shear stiffness properties.

useDensity: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether or not to use the value of density. The default value is OFF.

HomogeneousSolidSection#

class HomogeneousSolidSection(name, material, thickness=None)[source]#

The HomogeneousSolidSection object defines the properties of a solid section. The HomogeneousSolidSection object is derived from the SolidSection object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • SOLID SECTION

Note

Check HomogeneousSolidSection on help.3ds.com/0.1..

Public Data Attributes:

thickness

A Float specifying the thickness of the section.
Inherited from SolidSection

name

A String specifying the repository key.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

__init__(name, material[, thickness])

This method creates a HomogeneousSolidSection object.

setValues([thickness])

This method modifies the HomogeneousSolidSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
material: str[source]#

A String specifying the name of the material.

setValues(thickness=1)[source]#

This method modifies the HomogeneousSolidSection object.

Note

Check HomogeneousSolidSection.setValues on help.3ds.com/0.1..

Parameters:

thickness (float, default: 1) – A Float specifying the thickness of the section. Possible values are None or greater than zero. The default value is 1.0.

Raises:

RangeError –

thickness: Optional[float] = None[source]#

A Float specifying the thickness of the section. Possible values are None or greater than zero. The default value is 1.0.

Changed in version 2018: The default value is now 1.0 instead of None.

LayerProperties#

class LayerProperties(barArea, orientationAngle, layerName, material, barSpacing=0, layerPosition=0, spacingAngle=0, extensionRatio=0, radius=0)[source]#

The LayerProperties object defines the properties of a layer of reinforcement for membrane, shell, and surface sections.

Note

This object can be accessed by:

import section
mdb.models[name].parts[name].compositeLayups[i].section.rebarLayers.layerTable[i]
mdb.models[name].sections[name].rebarLayers.layerTable[i]
import odbSection
session.odbs[name].sections[name].rebarLayers.layerTable[i]

The corresponding analysis keywords are:

  • REBAR LAYER

Note

Check LayerProperties on help.3ds.com/0.1..

Public Data Attributes:

barSpacing

A Float specifying the spacing of the rebar.

layerPosition

A Float specifying the position of the rebar from the middle surface of the shell.

spacingAngle

A Float specifying the spacing angle of the rebar.

extensionRatio

A Float specifying the extension ratio for the rebar.

radius

A Float specifying the radius of the rebar.

Public Methods:

__init__(barArea, orientationAngle, ...[, ...])

This method creates a LayerProperties object.
barArea: float[source]#

A Float specifying the area per bar.

barSpacing: float = 0[source]#

A Float specifying the spacing of the rebar. This argument is only valid if the rebarSpacing argument on the parent RebarLayers object is set to CONSTANT. The default value is 0.0.

extensionRatio: float = 0[source]#

A Float specifying the extension ratio for the rebar. This argument is only valid if the rebarSpacing argument on the parent RebarLayers object is set to LIFT_EQUATION. The default value is 0.0.

layerName: str[source]#

A String specifying the name of the rebar layer.

layerPosition: float = 0[source]#

A Float specifying the position of the rebar from the middle surface of the shell. layerPosition applies only for homogeneous shell sections and composite shell sections. The default value is 0.0.

material: str[source]#

A String specifying the name of the rebar material.

orientationAngle: float[source]#

A Float or a String specifying the orientation of the rebar. A Float specifies the angular orientation; a String specifies an orientation name.

radius: float = 0[source]#

A Float specifying the radius of the rebar. This argument is only valid if the rebarSpacing argument on the parent RebarLayers object is set to LIFT_EQUATION. The default value is 0.0.

spacingAngle: float = 0[source]#

A Float specifying the spacing angle of the rebar. This argument is only valid if the rebarSpacing argument on the parent RebarLayers object is set to ANGULAR. The default value is 0.0.

LayerPropertiesArray#

LayerPropertiesArray[source]#

alias of List[LayerProperties]

MembraneSection#

class MembraneSection(name, material, thickness=1, thicknessType=abaqusConstants.UNIFORM, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, thicknessField='')[source]#

The MembraneSection object defines the properties of a membrane section. The MembraneSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • MEMBRANE SECTION

Note

Check MembraneSection on help.3ds.com/0.1..

Public Data Attributes:

rebarLayers

A RebarLayers object specifying reinforcement properties.

thickness

A Float specifying the thickness for the section.

thicknessType

A SymbolicConstant specifying the distribution used for defining the thickness of the elements.

poissonDefinition

A SymbolicConstant specifying whether to use the default value for the Poisson's ratio.

poisson

A Float specifying the section Poisson's ratio.

thicknessField

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

__init__(name, material[, thickness, ...])

This method creates a MembraneSection object.

setValues([thickness, thicknessType, ...])

This method modifies the MembraneSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
material: str[source]#

A String specifying the name of the material.

poisson: float = 0[source]#

A Float specifying the section Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

poissonDefinition: SymbolicConstant = DEFAULT[source]#

A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

rebarLayers: Optional[RebarLayers] = None[source]#

A RebarLayers object specifying reinforcement properties.

setValues(thickness=1, thicknessType=abaqusConstants.UNIFORM, poissonDefinition=abaqusConstants.DEFAULT, poisson=0, thicknessField='')[source]#

This method modifies the MembraneSection object.

Note

Check MembraneSection.setValues on help.3ds.com/0.1..

Parameters:

  • thickness (float, default: 1) – A Float specifying the thickness for the section. Possible values are thickness >> 0.0. The default value is 1.0.

  • thicknessType (SymbolicConstant, default: UNIFORM) – A SymbolicConstant specifying the distribution used for defining the thickness of the elements. Possible values are UNIFORM, ANALYTICAL_FIELD, and DISCRETE_FIELD. The default value is UNIFORM.

  • poissonDefinition (SymbolicConstant, default: DEFAULT) – A SymbolicConstant specifying whether to use the default value for the Poisson’s ratio. Possible values are:DEFAULT, specifying that the default value for the Poisson’s ratio is 0.5 in an Abaqus/Standard analysis and is obtained from the material definition in an Abaqus/Explicit analysis.VALUE, specifying that the Poisson’s ratio used in the analysis is the value provided in poisson.The default value is DEFAULT.

  • poisson (float, default: 0) – A Float specifying the section Poisson’s ratio. Possible values are −1.0 ≤ poisson ≤ 0.5. This argument is valid only when poissonDefinition = VALUE. The default value is 0.5.

  • thicknessField (str, default: '') – A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements. The thicknessField argument applies only when thicknessType = ANALYTICAL_FIELD or thicknessType = DISCRETE_FIELD. The default value is an empty string.

Raises:

RangeError –

thickness: float = 1[source]#

A Float specifying the thickness for the section. Possible values are thickness >> 0.0. The default value is 1.0.

thicknessField: str = ''[source]#

A String specifying the name of the AnalyticalField or DiscreteField object used to define the thickness of the shell elements. The thicknessField argument applies only when thicknessType = ANALYTICAL_FIELD or thicknessType = DISCRETE_FIELD. The default value is an empty string.

thicknessType: SymbolicConstant = UNIFORM[source]#

A SymbolicConstant specifying the distribution used for defining the thickness of the elements. Possible values are UNIFORM, ANALYTICAL_FIELD, and DISCRETE_FIELD. The default value is UNIFORM.

MPCSection#

class MPCSection(name, mpcType, userMode=abaqusConstants.DOF_MODE, userType=0)[source]#

The MPCSection object defines the properties of a multi-point constraint section. The MPCSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • MPC

Note

Check MPCSection on help.3ds.com/0.1..

Public Data Attributes:

userMode

A SymbolicConstant specifying the mode of the MPC when it is user-defined.

userType

An Int specifying to differentiate between different constraint types in a user-defined MPCSection.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

__init__(name, mpcType[, userMode, userType])

This method creates a MPCSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
mpcType: SymbolicConstant[source]#

A SymbolicConstant specifying the MPC type of the section. Possible values are BEAM_MPC, ELBOW_MPC, PIN_MPC, LINK_MPC, TIE_MPC, and USER_DEFINED.

userMode: SymbolicConstant = DOF_MODE[source]#

A SymbolicConstant specifying the mode of the MPC when it is user-defined. Possible values are DOF_MODE and NODE_MODE. The default value is DOF_MODE.The userMode argument applies only when mpcType = USER_DEFINED.

userType: int = 0[source]#

An Int specifying to differentiate between different constraint types in a user-defined MPCSection. The default value is 0.The userType argument applies only when mpcType = USER_DEFINED.

PEGSection#

class PEGSection(name, material, thickness=1, wedgeAngle1=0, wedgeAngle2=0)[source]#

The PEGSection object defines the properties of a solid section. The PEGSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • SOLID SECTION

Note

Check PEGSection on help.3ds.com/0.1..

Public Data Attributes:

thickness

A Float specifying the thickness of the section.

wedgeAngle1

A Float specifying the value of the x component of the angle between the bounding planes, ΔϕxΔ⁢ϕx.

wedgeAngle2

A Float specifying the value of the y component of the angle between the bounding planes, ΔϕyΔ⁢ϕy.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

__init__(name, material[, thickness, ...])

This method creates a PEGSection object.

setValues([thickness, wedgeAngle1, wedgeAngle2])

This method modifies the PEGSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
material: str[source]#

A String specifying the name of the material.

setValues(thickness=1, wedgeAngle1=0, wedgeAngle2=0)[source]#

This method modifies the PEGSection object.

Note

Check PEGSection.setValues on help.3ds.com/0.1..

Parameters:

  • thickness (float, default: 1) – A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

  • wedgeAngle1 (float, default: 0) – A Float specifying the value of the x component of the angle between the bounding planes, ΔϕxΔ⁢ϕx. The default value is 0.0.

  • wedgeAngle2 (float, default: 0) – A Float specifying the value of the y component of the angle between the bounding planes, ΔϕyΔ⁢ϕy. The default value is 0.0.

Raises:

RangeError –

thickness: float = 1[source]#

A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

wedgeAngle1: float = 0[source]#

A Float specifying the value of the x component of the angle between the bounding planes, ΔϕxΔ⁢ϕx. The default value is 0.0.

wedgeAngle2: float = 0[source]#

A Float specifying the value of the y component of the angle between the bounding planes, ΔϕyΔ⁢ϕy. The default value is 0.0.

RebarLayers#

class RebarLayers(rebarSpacing, layerTable)[source]#

The RebarLayers object defines the rebar properties of a section.

Note

This object can be accessed by:

import section
mdb.models[name].parts[name].compositeLayups[i].section.rebarLayers
mdb.models[name].sections[name].rebarLayers
import odbSection
session.odbs[name].sections[name].rebarLayers

The corresponding analysis keywords are:

  • REBAR LAYER

Note

Check RebarLayers on help.3ds.com/0.1..

Public Methods:

__init__(rebarSpacing, layerTable)

This method creates a RebarLayers object.

setValues(*args, **kwargs)

This method modifies the RebarLayers object.
layerTable: List[LayerProperties][source]#

A LayerPropertiesArray object specifying the layers of reinforcement.

rebarSpacing: SymbolicConstant[source]#

A SymbolicConstant specifying the type of rebar geometry. Possible values are CONSTANT, ANGULAR, and LIFT_EQUATION.

setValues(*args, **kwargs)[source]#

This method modifies the RebarLayers object.

SectionLayer#

class SectionLayer(thickness, material, orientAngle=0, numIntPts=3, axis=abaqusConstants.AXIS_3, angle=0, additionalRotationType=abaqusConstants.ROTATION_NONE, plyName='', orientation=None, additionalRotationField='')[source]#

The SectionLayer object defines the material layer in a composite shell.

Note

This object can be accessed by:

import section
mdb.models[name].parts[name].compositeLayups[i].section.layup[i]
mdb.models[name].sections[name].layup[i]
import odbSection
session.odbs[name].sections[name].layup[i]

The corresponding analysis keywords are:

  • SHELL SECTION

  • SHELL GENERAL SECTION

Changed in version 2017: The thicknessType attribute and thicknessField attribute were removed.

Note

Check SectionLayer on help.3ds.com/0.1..

Public Data Attributes:

orientAngle

A Float or a String specifying the relative orientation of the section layer.

numIntPts

An Int specifying the number of integration points to be used through the section.

axis

A SymbolicConstant specifying the axis of a cylindrical or spherical datum coordinate system about which an additional rotation is applied.

angle

A Float specifying the angle of the additional rotation.

additionalRotationType

A SymbolicConstant specifying the method used to describe the additional rotation when a valid orientation is specified.

plyName

A String specifying the ply identifier for this section layer.

orientation

The SymbolicConstant None or a DatumCsys object specifying a coordinate system reference for the relative orientation of this layer.

additionalRotationField

A String specifying the name of the field specifying the additional rotation.

Public Methods:

__init__(thickness, material[, orientAngle, ...])

This method creates a SectionLayer object.
additionalRotationField: str = ''[source]#

A String specifying the name of the field specifying the additional rotation. The default value is “”.

additionalRotationType: SymbolicConstant = ROTATION_NONE[source]#

A SymbolicConstant specifying the method used to describe the additional rotation when a valid orientation is specified. Possible values are ROTATION_NONE, ROTATION_ANGLE, and ROTATION_FIELD. The default value is ROTATION_NONE.

angle: float = 0[source]#

A Float specifying the angle of the additional rotation. This only applies if a valid reference is provided for the orientation. The default value is 0.0.

axis: SymbolicConstant = AXIS_3[source]#

A SymbolicConstant specifying the axis of a cylindrical or spherical datum coordinate system about which an additional rotation is applied. For shells this axis is also the shell normal. This only applies if a valid reference is provided for the orientation. Possible values are AXIS_1, AXIS_2, and AXIS_3. The default value is AXIS_3.

material: str[source]#

A String specifying the name of the section layer material.

numIntPts: int = 3[source]#

An Int specifying the number of integration points to be used through the section. This argument is valid only if the preIntegrate argument on the parent CompositeShellSection object is set to ON. The default value is 3.

orientAngle: float = 0[source]#

A Float or a String specifying the relative orientation of the section layer. A Float specifies the angular orientation; a String specifies a user-subroutine orientation name. If a String is specified, a user-subroutine orientation is used, otherwise the Float value is used as an angular orientation. The default value is 0.0.

orientation: Optional[SymbolicConstant] = None[source]#

The SymbolicConstant None or a DatumCsys object specifying a coordinate system reference for the relative orientation of this layer. If this reference is valid it is used as the relative orientation of the layer, otherwise the orientAngle is used as described. The default value is None.

plyName: str = ''[source]#

A String specifying the ply identifier for this section layer. The default value is “”.

thickness: float[source]#

A Float specifying the thickness of the section layer.

SectionLayerArray#

SectionLayerArray[source]#

alias of List[SectionLayer]

ShellSection#

class ShellSection[source]#

The ShellSection object defines the properties of a shell section. The ShellSection object is derived from the Section object. The ShellSection object has no explicit constructor and no methods or members. The ShellSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

Note

Check ShellSection on help.3ds.com/0.1..

Public Data Attributes:

name

A String specifying the repository key.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object specifying the transverse shear stiffness properties.

Public Methods:

Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
name: str = ''[source]#

A String specifying the repository key.

transverseShear: Optional[TransverseShearShell] = None[source]#

A TransverseShearShell object specifying the transverse shear stiffness properties.

SolidSection#

class SolidSection[source]#

The ShellSection object defines the properties of a shell section. The ShellSection object is derived from the Section object. The ShellSection object has no explicit constructor and no methods or members. The ShellSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

Note

Check SolidSection on help.3ds.com/0.1..

Public Data Attributes:

name

A String specifying the repository key.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
name: str = ''[source]#

A String specifying the repository key.

SurfaceSection#

class SurfaceSection(name, useDensity=OFF, density=0)[source]#

The SurfaceSection object defines the properties of a surface section. The SurfaceSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • SURFACE SECTION

Note

Check SurfaceSection on help.3ds.com/0.1..

Public Data Attributes:

rebarLayers

A RebarLayers object specifying reinforcement properties.

useDensity

A Boolean specifying whether or not to use the value of density.

density

A Float specifying the value of density to apply to this section.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

__init__(name[, useDensity, density])

This method creates a SurfaceSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
density: float = 0[source]#

A Float specifying the value of density to apply to this section. The default value is 0.0.

rebarLayers: Optional[RebarLayers] = None[source]#

A RebarLayers object specifying reinforcement properties.

useDensity: Union[AbaqusBoolean, bool] = OFF[source]#

A Boolean specifying whether or not to use the value of density. The default value is OFF.

TransverseShearBeam#

class TransverseShearBeam(scfDefinition, k23=None, k13=None, slendernessCompensation=0)[source]#

The TransverseShearBeam object defines the transverse shear stiffness properties of a beam section.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name].beamTransverseShear
import odbSection
session.odbs[name].sections[name].beamTransverseShear

The corresponding analysis keywords are:

  • TRANSVERSE SHEAR STIFFNESS

Note

Check TransverseShearBeam on help.3ds.com/0.1..

Public Data Attributes:

k23

None or a Float specifying the k23 shear stiffness of the section.

k13

None or a Float specifying the k13 shear stiffness of the section.

slendernessCompensation

The SymbolicConstant COMPUTED or a Float specifying the slenderness compensation factor of the section.

Public Methods:

__init__(scfDefinition[, k23, k13, ...])

This method creates a TransverseShearBeam object.

setValues(*args, **kwargs)

This method modifies the TransverseShearBeam object.
k13: Optional[float] = None[source]#

None or a Float specifying the k13 shear stiffness of the section. The default value is None.

k23: Optional[float] = None[source]#

None or a Float specifying the k23 shear stiffness of the section. The default value is None.

scfDefinition: SymbolicConstant[source]#

A SymbolicConstant specifying how slenderness compensation factor of the section is given. Possible values are ANALYSIS_DEFAULT, COMPUTED, and VALUE.

setValues(*args, **kwargs)[source]#

This method modifies the TransverseShearBeam object.

slendernessCompensation: Union[SymbolicConstant, float] = 0[source]#

The SymbolicConstant COMPUTED or a Float specifying the slenderness compensation factor of the section. The default value is 0.25.

TransverseShearShell#

class TransverseShearShell(k11, k22, k12)[source]#

The TransverseShearShell object defines the transverse shear stiffness properties of a shell section.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name].transverseShear
import odbSection
session.odbs[name].sections[name].transverseShear

The corresponding analysis keywords are:

  • TRANSVERSE SHEAR STIFFNESS

Note

Check TransverseShearShell on help.3ds.com/0.1..

Public Methods:

__init__(k11, k22, k12)

This method creates a TransverseShearShell object.

setValues(*args, **kwargs)

This method modifies the TransverseShearShell object.
k11: float[source]#

A Float specifying the shear stiffness of the section in the first direction.

k12: float[source]#

A Float specifying the coupling term in the shear stiffness of the section.

k22: float[source]#

A Float specifying the shear stiffness of the section in the second direction.

setValues(*args, **kwargs)[source]#

This method modifies the TransverseShearShell object.

TrussSection#

class TrussSection(name, material, area=1)[source]#

The TrussSection object defines the properties of a truss section. The TrussSection object is derived from the Section object.

Note

This object can be accessed by:

import section
mdb.models[name].sections[name]
import odbSection
session.odbs[name].sections[name]

The corresponding analysis keywords are:

  • SOLID SECTION

Note

Check TrussSection on help.3ds.com/0.1..

Public Data Attributes:

area

A Float specifying the cross-sectional area for the section.
Inherited from SectionBase

behaviorOptions

A ConnectorBehaviorOptionArray object.

name

A String specifying the repository key.

beamTransverseShear

A TransverseShearBeam object.

transverseShear

A TransverseShearShell object.

Public Methods:

__init__(name, material[, area])

This method creates a TrussSection object.

setValues([area])

This method modifies the TrussSection object.
Inherited from Section

TransverseShearBeam(scfDefinition[, k23, ...])

This method creates a TransverseShearBeam object.

TransverseShearShell(k11, k22, k12)

This method creates a TransverseShearShell object.
Inherited from ConnectorSection

ConnectorDamage([coupling, criterion, ...])

This method creates a connector damage behavior option for a ConnectorSection object.

ConnectorDamping([type, behavior, coupling, ...])

This method creates a connector damping behavior option for a ConnectorSection object.

ConnectorElasticity([behavior, coupling, ...])

This method creates a connector elasticity behavior option for a ConnectorSection object.

ConnectorFailure([releaseComponent, ...])

This method creates a connector failure behavior option for a ConnectorSection object.

ConnectorFriction([frictionModel, ...])

This method creates a connector friction behavior option for a ConnectorSection object.

ConnectorLock([lockingComponent, minMotion, ...])

This method creates a connector lock behavior option for a ConnectorSection.

ConnectorPlasticity([coupling, isotropic, ...])

This method creates a connector plasticity behavior option for a ConnectorSection object.

ConnectorPotential([componentStyle, ...])

This method creates a connector potential object to be used in conjunction with an allowable connector behavior option.

ConnectorStop([minMotion, maxMotion, components])

This method creates a connector stop behavior option for a ConnectorSection object.

DerivedComponent()

This method creates a DerivedComponent object.

TangentialBehavior([formulation, ...])

This method creates a TangentialBehavior object.
Inherited from SectionBase

sectionsFromOdb(fileName)

This method creates Section objects by reading an output database.
area: float = 1[source]#

A Float specifying the cross-sectional area for the section. Possible values are area >> 0. The default value is 1.0.

material: str[source]#

A String specifying the name of the material.

setValues(area=1)[source]#

This method modifies the TrussSection object.

Note

Check TrussSection.setValues on help.3ds.com/0.1..

Parameters:

area (float, default: 1) – A Float specifying the cross-sectional area for the section. Possible values are area >> 0. The default value is 1.0.

Raises:

RangeError –