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

Connector

Create sections#

In Mdb#

class SectionModel(name: str, description: str = '', stefanBoltzmann: float | None = None, absoluteZero: float | None = None, waveFormulation: SymbolicConstantType = 'NOT_SET', modelType: SymbolicConstantType = 'STANDARD_EXPLICIT', universalGas: float | None = None, copyConstraints: BooleanType = 1, copyConnectors: BooleanType = 1, copyInteractions: BooleanType = 1)[source]#

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

Notes

This object can be accessed by:

mdb.models[name]

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.
`MPCSection`(name, mpcType[, userMode, userType])	This method creates a MPCSection object.
`MembraneSection`(name, material[, thickness, ...])	This method creates a MembraneSection 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.

AcousticInfiniteSection(name: str, material: str, thickness: float = 1, order: int = 10) → AcousticInfiniteSection[source]#

This method creates an AcousticInfiniteSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
thickness: A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.
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. Possible values are 0 << order ≤≤ 10. The default value is 10.

Returns:

An AcousticInfiniteSection object.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

AcousticInterfaceSection(name: str, thickness: float = 1) → AcousticInterfaceSection[source]#

This method creates an AcousticInterfaceSection object.

Parameters:

name: A String specifying the repository key.
thickness: A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

Returns:

An AcousticInterfaceSection object.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

BeamSection(name: str, integration: SymbolicConstantType, profile: str, poissonRatio: float = 0, thermalExpansion: BooleanType = 0, temperatureDependency: BooleanType = 0, dependencies: int = 0, density: float | None = None, referenceTemperature: float | None = None, temperatureVar: SymbolicConstantType = 'LINEAR', alphaDamping: float = 0, betaDamping: float = 0, compositeDamping: float = 0, useFluidInertia: BooleanType = 0, submerged: SymbolicConstantType = 'FULLY', fluidMassDensity: float | None = None, crossSectionRadius: float | None = None, lateralMassCoef: float = 1, axialMassCoef: float = 0, massOffsetX: float = 0, massOffsetY: float = 0, beamShape: SymbolicConstantType = 'CONSTANT', material: str = '', table: tuple = (), outputPts: tuple = (), centroid: tuple[float] = (), shearCenter: tuple[float] = (), profileEnd: str = '') → BeamSection[source]#

This method creates a BeamSection object.

Parameters:

name: A String specifying the repository key.
integration: A SymbolicConstant specifying the integration method for the section. Possible values are BEFORE_ANALYSIS and DURING_ANALYSIS.
profile: A String specifying the name of the profile. This argument represents the start profile in case of *beamShape*=TAPERED.
poissonRatio: A Float specifying the Poisson’s ratio of the section. The default value is 0.0.
thermalExpansion: A Boolean specifying whether to use thermal expansion data. The default value is OFF.
temperatureDependency: A Boolean specifying whether the data depend on temperature. The default value is OFF.
dependencies: An Int specifying the number of field variable dependencies. The default value is 0.
density: None or a Float specifying the density of the section. The default value is None.
referenceTemperature: None or a Float specifying the reference temperature of the section. The default value is None.
temperatureVar: A SymbolicConstant specifying the temperature variation for the section. Possible values are LINEAR and INTERPOLATED. The default value is LINEAR.
alphaDamping: A Float specifying the αRαR factor to create mass proportional damping in direct-integration dynamics. The default value is 0.0.
betaDamping: A Float specifying the βRβR factor to create stiffness proportional damping in direct-integration dynamics. The default value is 0.0.
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). The default value is 0.0.
useFluidInertia: A Boolean specifying whether added mass effects will be simulated. The default value is OFF.
submerged: 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: 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: 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: 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: 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: 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: 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: 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: 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: A sequence of sequences of Floats specifying the items described below. The default value is an empty sequence.
outputPts: A sequence of pairs of Floats specifying the positions at which output is requested. The default value is an empty sequence.
centroid: A pair of Floats specifying the X–Y coordinates of the centroid. The default value is (0.0, 0.0).
shearCenter: A pair of Floats specifying the X–Y coordinates of the shear center. The default value is (0.0, 0.0).
profileEnd: 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.

Notes

This function can be accessed by:

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

CohesiveSection(name: str, response: SymbolicConstantType, material: str, initialThicknessType: SymbolicConstantType = 'SOLVER_DEFAULT', initialThickness: float = 1, outOfPlaneThickness: float | None = None) → CohesiveSection[source]#

This method creates a CohesiveSection object.

Parameters:

name: A String specifying the repository key.
response: A SymbolicConstant specifying the geometric assumption that defines the constitutive behavior of the cohesive elements. Possible values are TRACTION_SEPARATION, CONTINUUM, and GASKET.
material: A String specifying the name of the material.
initialThicknessType: 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: A Float specifying the initial thickness for the section. The initialThickness argument applies only when *initialThicknessType*=SPECIFY. The default value is 1.0.
outOfPlaneThickness: None or a Float specifying the out-of-plane thickness for the section. The default value is None.

Returns:

A CohesiveSection object.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

CompositeShellSection(name: str, layup: SectionLayerArray, symmetric: BooleanType = 0, thicknessType: SymbolicConstantType = 'UNIFORM', preIntegrate: BooleanType = 0, poissonDefinition: SymbolicConstantType = 'DEFAULT', poisson: float = 0, integrationRule: SymbolicConstantType = 'SIMPSON', temperature: SymbolicConstantType = 'GRADIENT', idealization: SymbolicConstantType = 'NO_IDEALIZATION', nTemp: int | None = None, thicknessModulus: float | None = None, useDensity: BooleanType = 0, density: float = 0, layupName: str = '', thicknessField: str = '', nodalThicknessField: str = '') → CompositeShellSection[source]#

This method creates a CompositeShellSection object.

Parameters:

name: A String specifying the repository key.
layup: A SectionLayerArray object specifying the shell cross-section.
symmetric: A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.
thicknessType: 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: 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: 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: 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: A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.
temperature: 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: 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: 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: 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: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.
layupName: A String specifying the layup name for this section. The default value is an empty string.
thicknessField: 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: 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.

Notes

This function can be accessed by:

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

CompositeSolidSection(name: str, layup: SectionLayerArray, symmetric: BooleanType = 0, layupName: str = '') → CompositeSolidSection[source]#

This method creates a CompositeSolidSection object.

Parameters:

name: A String specifying the repository key.
layup: A SectionLayerArray object specifying the solid cross-section.
symmetric: A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.
layupName: A String specifying the layup name for this section. The default value is an empty string.

Returns:

A CompositeSolidSection object.

Notes

This function can be accessed by:

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

ConnectorSection(name: str, assembledType: SymbolicConstantType = 'NONE', rotationalType: SymbolicConstantType = 'NONE', translationalType: SymbolicConstantType = 'NONE', integration: SymbolicConstantType = 'UNSPECIFIED', u1ReferenceLength: float | None = None, u2ReferenceLength: float | None = None, u3ReferenceLength: float | None = None, ur1ReferenceAngle: float | None = None, ur2ReferenceAngle: float | None = None, ur3ReferenceAngle: float | None = None, massPerLength: float | None = None, contactAngle: float | None = None, materialFlowFactor: float = 1, regularize: BooleanType = 1, defaultTolerance: BooleanType = 1, regularization: float = 0, extrapolation: SymbolicConstantType = 'CONSTANT', behaviorOptions: ConnectorBehaviorOptionArray | None = None) → ConnectorSection[source]#

This method creates a ConnectorSection object.

Parameters:

name: A String specifying the repository key.
assembledType: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: A ConnectorBehaviorOptionArray object.

Returns:

A ConnectorSection object.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

EulerianSection(name: str, data: str) → EulerianSection[source]#

This method creates a EulerianSection object.

Parameters:

name: A String specifying the repository key.
data: 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.

Notes

This function can be accessed by:

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

GasketSection(name: str, material: str, crossSection: float = 1, initialGap: float = 0, initialThickness: SymbolicConstantType | float = 'DEFAULT', initialVoid: float = 0, stabilizationStiffness: SymbolicConstantType | float = 'DEFAULT') → GasketSection[source]#

This method creates a GasketSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material of which the gasket is made or material that defines gasket behavior.
crossSection: 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: A Float specifying the initial gap. The default value is 0.0.
initialThickness: 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: A Float specifying the initial void. The default value is 0.0.
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. 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.

Notes

This function can be accessed by:

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

GeneralStiffnessSection(name: str, stiffnessMatrix: tuple, referenceTemperature: float | None = None, applyThermalStress: BooleanType = 0, temperatureDependency: BooleanType = 0, dependencies: int = 0, poissonDefinition: SymbolicConstantType = 'DEFAULT', poisson: float = 0, useDensity: BooleanType = 0, density: float = 0, thermalStresses: tuple = (), scalingData: tuple = ()) → GeneralStiffnessSection[source]#

This method creates a GeneralStiffnessSection object.

Parameters:

name: A String specifying the repository key.
stiffnessMatrix: 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: None or a Float specifying the reference temperature for thermal expansion. The default value is None.
applyThermalStress: A Boolean specifying whether or not the section stiffness varies with thermal stresses. The default value is OFF.
temperatureDependency: A Boolean specifying whether the data depend on temperature. The default value is OFF.
dependencies: An Int specifying the number of field variable dependencies. The default value is 0.
poissonDefinition: 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: 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: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.
thermalStresses: 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: 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.

Notes

This function can be accessed by:

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

HomogeneousShellSection(name: str, material: str, thickness: float = 0, numIntPts: int = 5, thicknessType: SymbolicConstantType = 'UNIFORM', preIntegrate: BooleanType = 0, poissonDefinition: SymbolicConstantType = 'DEFAULT', poisson: float = 0, integrationRule: SymbolicConstantType = 'SIMPSON', temperature: SymbolicConstantType = 'GRADIENT', idealization: SymbolicConstantType = 'NO_IDEALIZATION', nTemp: int | None = None, thicknessModulus: float | None = None, useDensity: BooleanType = 0, density: float = 0, thicknessField: str = '', nodalThicknessField: str = '') → HomogeneousShellSection[source]#

This method creates a HomogeneousShellSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the section material.
thickness: A Float specifying the thickness of the section. The thickness argument applies only when *thicknessType*=UNIFORM. The default value is 0.0.
numIntPts: 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: 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: 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: 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: 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: A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.
temperature: 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: 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: 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: 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: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.
thicknessField: 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: 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.

Notes

This function can be accessed by:

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

HomogeneousSolidSection(name: str, material: str, thickness: float = 1) → HomogeneousSolidSection[source]#

This method creates a HomogeneousSolidSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
thickness: A Float specifying the thickness of the section. Possible values are None or greater than zero. The default value is 1.0.

Returns:

A HomogeneousSolidSection object.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

MPCSection(name: str, mpcType: SymbolicConstantType, userMode: SymbolicConstantType = 'DOF_MODE', userType: int = 0) → MPCSection[source]#

This method creates a MPCSection object.

Parameters:

name: A String specifying the repository key.
mpcType: 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: 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: 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.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

MembraneSection(name: str, material: str, thickness: float = 1, thicknessType: SymbolicConstantType = 'UNIFORM', poissonDefinition: SymbolicConstantType = 'DEFAULT', poisson: float = 0, thicknessField: str = '') → MembraneSection[source]#

This method creates a MembraneSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
thickness: A Float specifying the thickness for the section. Possible values are thickness >> 0.0. The default value is 1.0.
thicknessType: 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: 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: 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: 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.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

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

This method creates a PEGSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
thickness: A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.
wedgeAngle1: 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: 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.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

SurfaceSection(name: str, useDensity: BooleanType = 0, density: float = 0) → SurfaceSection[source]#

This method creates a SurfaceSection object.

Parameters:

name: A String specifying the repository key.
useDensity: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.

Returns:

A SurfaceSection object.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

TrussSection(name: str, material: str, area: float = 1) → TrussSection[source]#

This method creates a TrussSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
area: 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.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

In Odb#

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

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.
`MPCSection`(name, mpcType[, userMode, userType])	This method creates a MPCSection object.
`MembraneSection`(name, material[, thickness, ...])	This method creates a MembraneSection 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.

AcousticInfiniteSection(name: str, material: str, thickness: float = 1, order: int = 10) → AcousticInfiniteSection[source]#

This method creates an AcousticInfiniteSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
thickness: A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.
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. Possible values are 0 << order ≤≤ 10. The default value is 10.

Returns:

An AcousticInfiniteSection object.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

AcousticInterfaceSection(name: str, thickness: float = 1) → AcousticInterfaceSection[source]#

This method creates an AcousticInterfaceSection object.

Parameters:

name: A String specifying the repository key.
thickness: A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

Returns:

An AcousticInterfaceSection object.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

This method creates a BeamSection object.

Parameters:

name: A String specifying the repository key.
integration: A SymbolicConstant specifying the integration method for the section. Possible values are BEFORE_ANALYSIS and DURING_ANALYSIS.
profile: A String specifying the name of the profile. This argument represents the start profile in case of *beamShape*=TAPERED.
poissonRatio: A Float specifying the Poisson’s ratio of the section. The default value is 0.0.
thermalExpansion: A Boolean specifying whether to use thermal expansion data. The default value is OFF.
temperatureDependency: A Boolean specifying whether the data depend on temperature. The default value is OFF.
dependencies: An Int specifying the number of field variable dependencies. The default value is 0.
density: None or a Float specifying the density of the section. The default value is None.
referenceTemperature: None or a Float specifying the reference temperature of the section. The default value is None.
temperatureVar: A SymbolicConstant specifying the temperature variation for the section. Possible values are LINEAR and INTERPOLATED. The default value is LINEAR.
alphaDamping: A Float specifying the αRαR factor to create mass proportional damping in direct-integration dynamics. The default value is 0.0.
betaDamping: A Float specifying the βRβR factor to create stiffness proportional damping in direct-integration dynamics. The default value is 0.0.
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). The default value is 0.0.
useFluidInertia: A Boolean specifying whether added mass effects will be simulated. The default value is OFF.
submerged: 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: 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: 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: 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: 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: 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: 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: 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: 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: A sequence of sequences of Floats specifying the items described below. The default value is an empty sequence.
outputPts: A sequence of pairs of Floats specifying the positions at which output is requested. The default value is an empty sequence.
centroid: A pair of Floats specifying the X–Y coordinates of the centroid. The default value is (0.0, 0.0).
shearCenter: A pair of Floats specifying the X–Y coordinates of the shear center. The default value is (0.0, 0.0).
profileEnd: 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.

Notes

This function can be accessed by:

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

This method creates a CohesiveSection object.

Parameters:

name: A String specifying the repository key.
response: A SymbolicConstant specifying the geometric assumption that defines the constitutive behavior of the cohesive elements. Possible values are TRACTION_SEPARATION, CONTINUUM, and GASKET.
material: A String specifying the name of the material.
initialThicknessType: 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: A Float specifying the initial thickness for the section. The initialThickness argument applies only when *initialThicknessType*=SPECIFY. The default value is 1.0.
outOfPlaneThickness: None or a Float specifying the out-of-plane thickness for the section. The default value is None.

Returns:

A CohesiveSection object.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

This method creates a CompositeShellSection object.

Parameters:

name: A String specifying the repository key.
layup: A SectionLayerArray object specifying the shell cross-section.
symmetric: A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.
thicknessType: 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: 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: 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: 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: A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.
temperature: 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: 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: 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: 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: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.
layupName: A String specifying the layup name for this section. The default value is an empty string.
thicknessField: 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: 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.

Notes

This function can be accessed by:

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

CompositeSolidSection(name: str, layup: SectionLayerArray, symmetric: BooleanType = 0, layupName: str = '') → CompositeSolidSection[source]#

This method creates a CompositeSolidSection object.

Parameters:

name: A String specifying the repository key.
layup: A SectionLayerArray object specifying the solid cross-section.
symmetric: A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.
layupName: A String specifying the layup name for this section. The default value is an empty string.

Returns:

A CompositeSolidSection object.

Notes

This function can be accessed by:

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

This method creates a ConnectorSection object.

Parameters:

name: A String specifying the repository key.
assembledType: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: A ConnectorBehaviorOptionArray object.

Returns:

A ConnectorSection object.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

EulerianSection(name: str, data: str) → EulerianSection[source]#

This method creates a EulerianSection object.

Parameters:

name: A String specifying the repository key.
data: 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.

Notes

This function can be accessed by:

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

This method creates a GasketSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material of which the gasket is made or material that defines gasket behavior.
crossSection: 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: A Float specifying the initial gap. The default value is 0.0.
initialThickness: 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: A Float specifying the initial void. The default value is 0.0.
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. 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.

Notes

This function can be accessed by:

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

This method creates a GeneralStiffnessSection object.

Parameters:

name: A String specifying the repository key.
stiffnessMatrix: 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: None or a Float specifying the reference temperature for thermal expansion. The default value is None.
applyThermalStress: A Boolean specifying whether or not the section stiffness varies with thermal stresses. The default value is OFF.
temperatureDependency: A Boolean specifying whether the data depend on temperature. The default value is OFF.
dependencies: An Int specifying the number of field variable dependencies. The default value is 0.
poissonDefinition: 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: 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: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.
thermalStresses: 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: 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.

Notes

This function can be accessed by:

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

This method creates a HomogeneousShellSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the section material.
thickness: A Float specifying the thickness of the section. The thickness argument applies only when *thicknessType*=UNIFORM. The default value is 0.0.
numIntPts: 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: 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: 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: 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: 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: A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.
temperature: 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: 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: 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: 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: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.
thicknessField: 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: 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.

Notes

This function can be accessed by:

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

HomogeneousSolidSection(name: str, material: str, thickness: float = 1) → HomogeneousSolidSection[source]#

This method creates a HomogeneousSolidSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
thickness: A Float specifying the thickness of the section. Possible values are None or greater than zero. The default value is 1.0.

Returns:

A HomogeneousSolidSection object.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

MPCSection(name: str, mpcType: SymbolicConstantType, userMode: SymbolicConstantType = 'DOF_MODE', userType: int = 0) → MPCSection[source]#

This method creates a MPCSection object.

Parameters:

name: A String specifying the repository key.
mpcType: 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: 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: 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.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

This method creates a MembraneSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
thickness: A Float specifying the thickness for the section. Possible values are thickness >> 0.0. The default value is 1.0.
thicknessType: 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: 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: 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: 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.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

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

This method creates a PEGSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
thickness: A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.
wedgeAngle1: 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: 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.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

SurfaceSection(name: str, useDensity: BooleanType = 0, density: float = 0) → SurfaceSection[source]#

This method creates a SurfaceSection object.

Parameters:

name: A String specifying the repository key.
useDensity: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.

Returns:

A SurfaceSection object.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

TrussSection(name: str, material: str, area: float = 1) → TrussSection[source]#

This method creates a TrussSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
area: 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.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

Object features#

Section#

class Section[source]#

Methods

`TransverseShearBeam`(scfDefinition[, k23, ...])	This method creates a TransverseShearBeam object.
`TransverseShearShell`(k11, k22, k12)	This method creates a TransverseShearShell object.

ConnectorDamage(coupling: SymbolicConstantType = 'UNCOUPLED', criterion: SymbolicConstantType = 'FORCE', initiationTemperature: BooleanType = 0, initiationPotentialOperator: SymbolicConstantType = 'SUM', initiationPotentialExponent: float = 2, initiationDependencies: int = 0, evolution: BooleanType = 1, evolutionType: SymbolicConstantType = 'MOTION_TYPE', softening: SymbolicConstantType = 'LINEAR', useAffected: BooleanType = 0, degradation: SymbolicConstantType = 'MAXIMUM', evolutionTemperature: BooleanType = 0, evolutionDependencies: int = 0, evolutionPotentialOperator: SymbolicConstantType = 'SUM', evolutionPotentialExponent: float = 2, initiationPotentials: ConnectorPotentialArray | None = None, evolutionPotentials: ConnectorPotentialArray | None = None, initiationTable: tuple = (), evolutionTable: tuple = (), affectedComponents: tuple = (), components: tuple = ())[source]#

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

Parameters:

coupling: A SymbolicConstant specifying whether or not the behavior is coupled. Possible values are UNCOUPLED and COUPLED. The default value is UNCOUPLED.
criterion: A SymbolicConstant specifying the damage initiation criterion to be used. Possible values are FORCE, MOTION, and PLASTIC_MOTION. The default value is FORCE.
initiationTemperature: A Boolean specifying whether the initiation data depend on temperature. The default value is OFF.
initiationPotentialOperator: 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: 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: An Int specifying the number of field variable dependencies for the initiation data. The default value is 0.
evolution: A Boolean specifying whether damage evolution data will be used. The default value is ON.
evolutionType: 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: 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: 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: 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: A Boolean specifying whether the evolution data depend on temperature. The default value is OFF.This argument is applicable only if *evolution*=ON.
evolutionDependencies: 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: 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: 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: 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: 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: 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: 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: 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: 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.

Raises:

ValueError and TextError.

Notes

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorDamage
import odbConnectorBehavior
odbConnectorBehavior.ConnectorDamage

ConnectorDamping(behavior: SymbolicConstantType = 'LINEAR', coupling: SymbolicConstantType = 'UNCOUPLED', dependencies: int = 0, temperatureDependency: BooleanType = 0, frequencyDependency: BooleanType = 0, table: tuple = (), independentComponents: tuple = (), components: tuple = ())[source]#

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

Parameters:

behavior: A SymbolicConstant specifying if the damping behavior is linear or nonlinear. Possible values are LINEAR and NONLINEAR. The default value is LINEAR.
coupling: 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: An Int specifying the number of field variable dependencies. The default value is 0.
temperatureDependency: A Boolean specifying whether the behavior data depend on temperature. The default value is OFF.
frequencyDependency: 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: 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: 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: 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.

Raises:

ValueError and TextError.

Notes

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorDamping
import odbConnectorBehavior
odbConnectorBehavior.ConnectorDamping

ConnectorElasticity(behavior: SymbolicConstantType = 'LINEAR', coupling: SymbolicConstantType = 'UNCOUPLED', dependencies: int = 0, temperatureDependency: BooleanType = 0, frequencyDependency: BooleanType = 0, table: tuple = (), independentComponents: tuple = (), components: tuple = ())[source]#

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

Parameters:

behavior: 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: 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: An Int specifying the number of field variable dependencies. The default value is 0.This argument is not applicable if *behavior*=RIGID.
temperatureDependency: A Boolean specifying whether the behavior data depend on temperature. The default value is OFF.This argument is not applicable if *behavior*=RIGID.
frequencyDependency: 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: 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: 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: 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.

Raises:

ValueError and TextError.

Notes

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorElasticity
import odbConnectorBehavior
odbConnectorBehavior.ConnectorElasticity

ConnectorFailure(releaseComponent: SymbolicConstantType = 'ALL', minMotion: float | None = None, maxMotion: float | None = None, minForce: float | None = None, maxForce: float | None = None, components: tuple = ())[source]#

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

Parameters:

releaseComponent: 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: 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: 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: 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: 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: 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.

Raises:

ValueError and TextError.

Notes

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorFailure
import odbConnectorBehavior
odbConnectorBehavior.ConnectorFailure

ConnectorFriction(frictionModel: SymbolicConstantType = 'PREDEFINED', slipStyle: SymbolicConstantType = 'SPECIFY', tangentDirection: int | None = None, stickStiffness: float | None = None, componentType: SymbolicConstantType = 'NO_INDEPENDENT_COMPONENTS', slipDependency: BooleanType = 0, temperatureDependency: BooleanType = 0, dependencies: int = 0, useContactForceComponent: BooleanType = 0, contactForceStyle: SymbolicConstantType = 'COMPONENT_NUMBER', contactForceComponent: int = 0, forcePotentialOperator: SymbolicConstantType = 'SUM', forcePotentialExponent: float = 2, connectorPotentials: ConnectorPotentialArray | None = None, table: tuple = (), independentComponents: tuple = ())[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.

Parameters:

frictionModel: A SymbolicConstant specifying the desired frictional response model. Possible values are PREDEFINED and USER_CUSTOMIZED. The default value is PREDEFINED.
slipStyle: 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: 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: 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: 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: 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: A Boolean specifying whether the table data depend on temperature. The default value is OFF.This argument applies only if *frictionModel*=USER_CUSTOMIZED.
dependencies: An Int specifying the number of field variable dependencies. The default value is 0.This argument applies only if *frictionModel*=USER_CUSTOMIZED.
useContactForceComponent: 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: 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: 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: 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: 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: 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: 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: 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.

Raises:

ValueError and TextError.

Notes

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorFriction
import odbConnectorBehavior
odbConnectorBehavior.ConnectorFriction

ConnectorLock(lockingComponent: SymbolicConstantType = 'ALL', minMotion: float | None = None, maxMotion: float | None = None, minForce: float | None = None, maxForce: float | None = None, components: tuple = ())[source]#

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

Parameters:

lockingComponent: 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: 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: 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: 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: 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: 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.

Raises:

ValueError and TextError.

Notes

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorLock
import odbConnectorBehavior
odbConnectorBehavior.ConnectorLock

ConnectorPlasticity(coupling: SymbolicConstantType = 'UNCOUPLED', isotropic: BooleanType = 1, isotropicType: SymbolicConstantType = 'TABULAR', isotropicTemperature: BooleanType = 0, isotropicDependencies: int = 0, kinematic: BooleanType = 0, kinematicType: SymbolicConstantType = 'HALF_CYCLE', kinematicTemperature: BooleanType = 0, kinematicDependencies: int = 0, forcePotentialOperator: SymbolicConstantType = 'SUM', forcePotentialExponent: float = 2, connectorPotentials: ConnectorPotentialArray | None = None, isotropicTable: tuple = (), kinematicTable: tuple = (), components: tuple = ())[source]#

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

Parameters:

coupling: A SymbolicConstant specifying whether or not the behavior is coupled. Possible values are UNCOUPLED and COUPLED. The default value is UNCOUPLED.
isotropic: 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: 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: A Boolean specifying whether the isotropic data depend on temperature. The default value is OFF.This argument is applicable only if *isotropic*=ON.
isotropicDependencies: 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: 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: 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: A Boolean specifying whether the kinematic data depend on temperature. The default value is OFF.This argument is applicable only if *kinematic*=ON.
kinematicDependencies: 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: 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: 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: A ConnectorPotentialArray object specifying one ConnectorPotential object for each force potential contribution. This member can be specified only if *coupling*=COUPLED.
isotropicTable: 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: 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: 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.

Raises:

ValueError and TextError.

Notes

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorPlasticity
import odbConnectorBehavior
odbConnectorBehavior.ConnectorPlasticity

ConnectorPotential(componentStyle: SymbolicConstantType = 'COMPONENT_NUMBER', componentNumber: int = 0, sign: SymbolicConstantType = 'POSITIVE', scaleFactor: float = 1, positiveExponent: float = 2, shiftFactor: float = 0, hFunction: SymbolicConstantType = 'ABS')[source]#

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

Parameters:

componentStyle: 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: 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: A SymbolicConstant specifying the sign of the contribution. Possible values are POSITIVE and NEGATIVE. The default value is POSITIVE.
scaleFactor: A Float specifying the scaling factor for the contribution. The default value is 1.0.
positiveExponent: 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: A Float specifying the shift factor for the contribution. The default value is 0.0.
hFunction: 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.

Raises:

ValueError and TextError.

Notes

This function can be accessed by:

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

ConnectorStop(minMotion: float | None = None, maxMotion: float | None = None, components: tuple = ())[source]#

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

Parameters:

minMotion: 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: 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: 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.

Raises:

ValueError and TextError.

Notes

This function can be accessed by:

import connectorBehavior
connectorBehavior.ConnectorStop
import odbConnectorBehavior
odbConnectorBehavior.ConnectorStop

DerivedComponent()[source]#

This method creates a DerivedComponent object.

Returns:

A DerivedComponent object.

Raises:

ValueError and TextError.

Notes

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

TangentialBehavior(formulation: SymbolicConstantType = 'PENALTY', slipRateDependency: BooleanType = 0, pressureDependency: BooleanType = 0, temperatureDependency: BooleanType = 0, dependencies: int = 0, exponentialDecayDefinition: SymbolicConstantType = 'COEFFICIENTS', shearStressLimit: float | None = None, maximumElasticSlip: SymbolicConstantType = 'FRACTION', fraction: float | None = None, absoluteDistance: float | None = None, table: tuple = ())[source]#

This method creates a TangentialBehavior object.

Parameters:

formulation: A SymbolicConstant specifying the friction coefficient formulation. Possible values are PENALTY and EXPONENTIAL_DECAY. The default value is PENALTY.
slipRateDependency: A Boolean specifying whether the data depend on slip rate. The default value is OFF.
pressureDependency: A Boolean specifying whether the data depend on contact pressure. The default value is OFF.
temperatureDependency: A Boolean specifying whether the data depend on temperature. The default value is OFF.
dependencies: An Int specifying the number of field variables for the data. The default value is 0.
exponentialDecayDefinition: A SymbolicConstant specifying the exponential decay definition for the data. Possible values are COEFFICIENTS and TEST_DATA. The default value is COEFFICIENTS.
shearStressLimit: None or a Float specifying no upper limit or the friction coefficient shear stress limit. The default value is None.
maximumElasticSlip: 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: 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: 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: 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. .

Notes

This function can be accessed by:

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

TransverseShearBeam(scfDefinition: SymbolicConstantType, k23: float | None = None, k13: float | None = None, slendernessCompensation: SymbolicConstantType | float = 0) → TransverseShearBeam[source]#

This method creates a TransverseShearBeam object.

Parameters:

scfDefinition: A SymbolicConstant specifying how slenderness compensation factor of the section is given. Possible values are ANALYSIS_DEFAULT, COMPUTED, and VALUE.
k23: None or a Float specifying the k23 shear stiffness of the section. The default value is None.
k13: None or a Float specifying the k13 shear stiffness of the section. The default value is None.
slendernessCompensation: The SymbolicConstant COMPUTED or a Float specifying the slenderness compensation factor of the section. The default value is 0.25.

Returns:

A TransverseShearBeam object.

Notes

This function can be accessed by:

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

TransverseShearShell(k11: float, k22: float, k12: float) → TransverseShearShell[source]#

This method creates a TransverseShearShell object.

Parameters:

k11: A Float specifying the shear stiffness of the section in the first direction.
k22: A Float specifying the shear stiffness of the section in the second direction.
k12: A Float specifying the coupling term in the shear stiffness of the section.

Returns:

A TransverseShearShell object.

Notes

This function can be accessed by:

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

sectionsFromOdb(fileName: str)[source]#

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

Parameters:

fileName: 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 python:list of Section objects.

Notes

This function can be accessed by:

mdb.models[name].sectionsFromOdb

AcousticInfiniteSection#

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

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

Notes

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

Methods

setValues([thickness, order])

This method modifies the AcousticInfiniteSection object.

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

This method modifies the AcousticInfiniteSection object.

Parameters:

thickness: A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.
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. Possible values are 0 << order ≤≤ 10. The default value is 10.

Raises:

RangeError

AcousticInterfaceSection#

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

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

Notes

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

Methods

setValues([thickness])

This method modifies the AcousticInterfaceSection object.

setValues(thickness: float = 1)[source]#

This method modifies the AcousticInterfaceSection object.

Parameters:

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

Raises:

RangeError

BeamSection#

class BeamSection(name: str, integration: SymbolicConstantType, profile: str, poissonRatio: float = 0, thermalExpansion: BooleanType = 0, temperatureDependency: BooleanType = 0, dependencies: int = 0, density: float | None = None, referenceTemperature: float | None = None, temperatureVar: SymbolicConstantType = 'LINEAR', alphaDamping: float = 0, betaDamping: float = 0, compositeDamping: float = 0, useFluidInertia: BooleanType = 0, submerged: SymbolicConstantType = 'FULLY', fluidMassDensity: float | None = None, crossSectionRadius: float | None = None, lateralMassCoef: float = 1, axialMassCoef: float = 0, massOffsetX: float = 0, massOffsetY: float = 0, beamShape: SymbolicConstantType = 'CONSTANT', material: str = '', table: tuple = (), outputPts: tuple = (), centroid: tuple[float] = (), shearCenter: tuple[float] = (), profileEnd: str = '')[source]#

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

Notes

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:
The table data specify the following:
    - 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

Attributes:

beamTransverseShear: TransverseShearBeam: A TransverseShearBeam object specifying the transverse shear stiffness properties.

Methods

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

This method modifies the BeamSection object.

setValues(poissonRatio: float = 0, thermalExpansion: BooleanType = 0, temperatureDependency: BooleanType = 0, dependencies: int = 0, density: float | None = None, referenceTemperature: float | None = None, temperatureVar: SymbolicConstantType = 'LINEAR', alphaDamping: float = 0, betaDamping: float = 0, compositeDamping: float = 0, useFluidInertia: BooleanType = 0, submerged: SymbolicConstantType = 'FULLY', fluidMassDensity: float | None = None, crossSectionRadius: float | None = None, lateralMassCoef: float = 1, axialMassCoef: float = 0, massOffsetX: float = 0, massOffsetY: float = 0, beamShape: SymbolicConstantType = 'CONSTANT', material: str = '', table: tuple = (), outputPts: tuple = (), centroid: tuple[float] = (), shearCenter: tuple[float] = (), profileEnd: str = '')[source]#

This method modifies the BeamSection object.

Parameters:

poissonRatio: A Float specifying the Poisson’s ratio of the section. The default value is 0.0.
thermalExpansion: A Boolean specifying whether to use thermal expansion data. The default value is OFF.
temperatureDependency: A Boolean specifying whether the data depend on temperature. The default value is OFF.
dependencies: An Int specifying the number of field variable dependencies. The default value is 0.
density: None or a Float specifying the density of the section. The default value is None.
referenceTemperature: None or a Float specifying the reference temperature of the section. The default value is None.
temperatureVar: A SymbolicConstant specifying the temperature variation for the section. Possible values are LINEAR and INTERPOLATED. The default value is LINEAR.
alphaDamping: A Float specifying the αRαR factor to create mass proportional damping in direct-integration dynamics. The default value is 0.0.
betaDamping: A Float specifying the βRβR factor to create stiffness proportional damping in direct-integration dynamics. The default value is 0.0.
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). The default value is 0.0.
useFluidInertia: A Boolean specifying whether added mass effects will be simulated. The default value is OFF.
submerged: 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: 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: 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: 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: 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: 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: 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: 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: 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: A sequence of sequences of Floats specifying the items described below. The default value is an empty sequence.
outputPts: A sequence of pairs of Floats specifying the positions at which output is requested. The default value is an empty sequence.
centroid: A pair of Floats specifying the X–Y coordinates of the centroid. The default value is (0.0, 0.0).
shearCenter: A pair of Floats specifying the X–Y coordinates of the shear center. The default value is (0.0, 0.0).
profileEnd: 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.

CohesiveSection#

class CohesiveSection(name: str, response: SymbolicConstantType, material: str, initialThicknessType: SymbolicConstantType = 'SOLVER_DEFAULT', initialThickness: float = 1, outOfPlaneThickness: float | None = None)[source]#

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

Notes

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

Methods

setValues([initialThicknessType, ...])

This method modifies the CohesiveSection object.

setValues(initialThicknessType: SymbolicConstantType = 'SOLVER_DEFAULT', initialThickness: float = 1, outOfPlaneThickness: float | None = None)[source]#

This method modifies the CohesiveSection object.

Parameters:

initialThicknessType: 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: A Float specifying the initial thickness for the section. The initialThickness argument applies only when *initialThicknessType*=SPECIFY. The default value is 1.0.
outOfPlaneThickness: None or a Float specifying the out-of-plane thickness for the section. The default value is None.

Raises:

RangeError

CompositeShellSection#

class CompositeShellSection(name: str, layup: SectionLayerArray, symmetric: BooleanType = 0, thicknessType: SymbolicConstantType = 'UNIFORM', preIntegrate: BooleanType = 0, poissonDefinition: SymbolicConstantType = 'DEFAULT', poisson: float = 0, integrationRule: SymbolicConstantType = 'SIMPSON', temperature: SymbolicConstantType = 'GRADIENT', idealization: SymbolicConstantType = 'NO_IDEALIZATION', nTemp: int | None = None, thicknessModulus: float | None = None, useDensity: BooleanType = 0, density: float = 0, layupName: str = '', thicknessField: str = '', nodalThicknessField: str = '')[source]#

The CompositeShellSection object defines the properties of a composite shell section. The CompositeShellSection object is derived from the GeometryShellSection object.

Notes

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

Attributes:

rebarLayers: RebarLayers: A RebarLayers object specifying reinforcement properties.
transverseShear: TransverseShearShell: A TransverseShearShell object specifying the transverse shear stiffness properties.

Methods

setValues([symmetric, thicknessType, ...])

This method modifies the CompositeShellSection object.

rebarLayers: RebarLayers = None[source]#

setValues(symmetric: BooleanType = 0, thicknessType: SymbolicConstantType = 'UNIFORM', preIntegrate: BooleanType = 0, poissonDefinition: SymbolicConstantType = 'DEFAULT', poisson: float = 0, integrationRule: SymbolicConstantType = 'SIMPSON', temperature: SymbolicConstantType = 'GRADIENT', idealization: SymbolicConstantType = 'NO_IDEALIZATION', nTemp: int | None = None, thicknessModulus: float | None = None, useDensity: BooleanType = 0, density: float = 0, layupName: str = '', thicknessField: str = '', nodalThicknessField: str = '')[source]#

This method modifies the CompositeShellSection object.

Parameters:

symmetric: A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.
thicknessType: 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: 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: 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: 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: A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.
temperature: 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: 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: 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: 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: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.
layupName: A String specifying the layup name for this section. The default value is an empty string.
thicknessField: 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: 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.

transverseShear: TransverseShearShell = None[source]#

CompositeSolidSection#

class CompositeSolidSection(name: str, layup: SectionLayerArray, symmetric: BooleanType = 0, layupName: str = '')[source]#

The CompositeSolidSection object defines the properties of a composite solid section. The CompositeSolidSection object is derived from the Section object.

Notes

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

Methods

setValues([symmetric, layupName])

This method modifies the CompositeSolidSection object.

setValues(symmetric: BooleanType = 0, layupName: str = '')[source]#

This method modifies the CompositeSolidSection object.

Parameters:

symmetric: A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.
layupName: A String specifying the layup name for this section. The default value is an empty string.

ConnectorSection#

class ConnectorSection(name: str, assembledType: SymbolicConstantType = 'NONE', rotationalType: SymbolicConstantType = 'NONE', translationalType: SymbolicConstantType = 'NONE', integration: SymbolicConstantType = 'UNSPECIFIED', u1ReferenceLength: float | None = None, u2ReferenceLength: float | None = None, u3ReferenceLength: float | None = None, ur1ReferenceAngle: float | None = None, ur2ReferenceAngle: float | None = None, ur3ReferenceAngle: float | None = None, massPerLength: float | None = None, contactAngle: float | None = None, materialFlowFactor: float = 1, regularize: BooleanType = 1, defaultTolerance: BooleanType = 1, regularization: float = 0, extrapolation: SymbolicConstantType = 'CONSTANT', behaviorOptions: ConnectorBehaviorOptionArray | None = None)[source]#

A ConnectorSection object describes the connection type and the behavior of a connector. The ConnectorSection object is derived from the Section object.

Notes

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

Methods

setValues([assembledType, rotationalType, ...])

This method modifies the ConnectorSection object.

setValues(assembledType: SymbolicConstantType = 'NONE', rotationalType: SymbolicConstantType = 'NONE', translationalType: SymbolicConstantType = 'NONE', integration: SymbolicConstantType = 'UNSPECIFIED', u1ReferenceLength: float | None = None, u2ReferenceLength: float | None = None, u3ReferenceLength: float | None = None, ur1ReferenceAngle: float | None = None, ur2ReferenceAngle: float | None = None, ur3ReferenceAngle: float | None = None, massPerLength: float | None = None, contactAngle: float | None = None, materialFlowFactor: float = 1, regularize: BooleanType = 1, defaultTolerance: BooleanType = 1, regularization: float = 0, extrapolation: SymbolicConstantType = 'CONSTANT', behaviorOptions: ConnectorBehaviorOptionArray | None = None)[source]#

This method modifies the ConnectorSection object.

Parameters:

assembledType: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: A ConnectorBehaviorOptionArray object.

Raises:

RangeError

EulerianSection#

class EulerianSection(name: str, data: str)[source]#

The EulerianSection object defines the properties of a Eulerian section. The EulerianSection object is derived from the Section object.

Notes

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

Methods

setValues()

This method modifies the EulerianSection object.

setValues()[source]#: This method modifies the EulerianSection object.

GasketSection#

class GasketSection(name: str, material: str, crossSection: float = 1, initialGap: float = 0, initialThickness: SymbolicConstantType | float = 'DEFAULT', initialVoid: float = 0, stabilizationStiffness: SymbolicConstantType | float = 'DEFAULT')[source]#

The GasketSection object defines the properties of a gasket section. The GasketSection object is derived from the Section object.

Notes

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

Methods

setValues([crossSection, initialGap, ...])

This method modifies the GasketSection object.

setValues(crossSection: float = 1, initialGap: float = 0, initialThickness: SymbolicConstantType | float = 'DEFAULT', initialVoid: float = 0, stabilizationStiffness: SymbolicConstantType | float = 'DEFAULT')[source]#

This method modifies the GasketSection object.

Parameters:

crossSection: 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: A Float specifying the initial gap. The default value is 0.0.
initialThickness: 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: A Float specifying the initial void. The default value is 0.0.
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. 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.

GeneralStiffnessSection#

class GeneralStiffnessSection(name: str, stiffnessMatrix: tuple, referenceTemperature: float | None = None, applyThermalStress: BooleanType = 0, temperatureDependency: BooleanType = 0, dependencies: int = 0, poissonDefinition: SymbolicConstantType = 'DEFAULT', poisson: float = 0, useDensity: BooleanType = 0, density: float = 0, thermalStresses: tuple = (), scalingData: tuple = ())[source]#

The GeneralStiffnessSection object defines the properties of a shell section via the stiffness matrix. The GeneralStiffnessSection object is derived from the ShellSection object.

Notes

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

Attributes:

rebarLayers: RebarLayers: A RebarLayers object specifying reinforcement properties.
transverseShear: TransverseShearShell: A TransverseShearShell object specifying the transverse shear stiffness properties.

Methods

setValues([referenceTemperature, ...])

This method modifies the GeneralStiffnessSection object.

setValues(referenceTemperature: float | None = None, applyThermalStress: BooleanType = 0, temperatureDependency: BooleanType = 0, dependencies: int = 0, poissonDefinition: SymbolicConstantType = 'DEFAULT', poisson: float = 0, useDensity: BooleanType = 0, density: float = 0, thermalStresses: tuple = (), scalingData: tuple = ())[source]#

This method modifies the GeneralStiffnessSection object.

Parameters:

referenceTemperature: None or a Float specifying the reference temperature for thermal expansion. The default value is None.
applyThermalStress: A Boolean specifying whether or not the section stiffness varies with thermal stresses. The default value is OFF.
temperatureDependency: A Boolean specifying whether the data depend on temperature. The default value is OFF.
dependencies: An Int specifying the number of field variable dependencies. The default value is 0.
poissonDefinition: 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: 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: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.
thermalStresses: 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: 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.

transverseShear: TransverseShearShell = None[source]#

GeometryShellSection#

class GeometryShellSection(nodalThicknessField: str = '', thicknessField: str = '', thicknessType: SymbolicConstantType = 'UNIFORM', preIntegrate: BooleanType = 0, poissonDefinition: SymbolicConstantType = 'DEFAULT', poisson: float = 0, integrationRule: SymbolicConstantType = 'SIMPSON', temperature: SymbolicConstantType = 'GRADIENT', nTemp: int | None = None, thicknessModulus: float | None = None, useDensity: BooleanType = 0, density: float = 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.

Notes

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]

Attributes:

name: str: A String specifying the repository key.
thicknessType: SymbolicConstant: 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: Boolean: 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: 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: 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: A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.
temperature: SymbolicConstant: 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: 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: int: 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: float: 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: Boolean: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: float: A Float specifying the value of density to apply to this section. The default value is 0.0.
thicknessField: str: 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.
rebarLayers: RebarLayers: A RebarLayers object specifying reinforcement properties.
nodalThicknessField: str: 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.
transverseShear: TransverseShearShell: A TransverseShearShell object specifying the transverse shear stiffness properties.

Methods

RebarLayers(rebarSpacing, layerTable)

This method creates a RebarLayers object.

RebarLayers(rebarSpacing: SymbolicConstantType, layerTable: LayerPropertiesArray) → RebarLayers[source]#

This method creates a RebarLayers object.

Parameters:

rebarSpacing: A SymbolicConstant specifying the type of rebar geometry. Possible values are CONSTANT, ANGULAR, and LIFT_EQUATION.
layerTable: A LayerPropertiesArray object specifying the layers of reinforcement.

Returns:

A RebarLayers object.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].compositeLayups[*name*].Section

transverseShear: TransverseShearShell = None[source]#

HomogeneousShellSection#

class HomogeneousShellSection(name: str, material: str, thickness: float = 0, numIntPts: int = 5, thicknessType: SymbolicConstantType = 'UNIFORM', preIntegrate: BooleanType = 0, poissonDefinition: SymbolicConstantType = 'DEFAULT', poisson: float = 0, integrationRule: SymbolicConstantType = 'SIMPSON', temperature: SymbolicConstantType = 'GRADIENT', idealization: SymbolicConstantType = 'NO_IDEALIZATION', nTemp: int | None = None, thicknessModulus: float | None = None, useDensity: BooleanType = 0, density: float = 0, thicknessField: str = '', nodalThicknessField: str = '')[source]#

The HomogeneousShellSection object defines the properties of a shell section. The HomogeneousShellSection object is derived from the GeometryShellSection object.

Notes

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

Attributes:

rebarLayers: RebarLayers: A RebarLayers object specifying reinforcement properties.
transverseShear: TransverseShearShell: A TransverseShearShell object specifying the transverse shear stiffness properties.

Methods

setValues([thickness, numIntPts, ...])

This method modifies the HomogeneousShellSection object.

rebarLayers: RebarLayers = None[source]#

setValues(thickness: float = 0, numIntPts: int = 5, thicknessType: SymbolicConstantType = 'UNIFORM', preIntegrate: BooleanType = 0, poissonDefinition: SymbolicConstantType = 'DEFAULT', poisson: float = 0, integrationRule: SymbolicConstantType = 'SIMPSON', temperature: SymbolicConstantType = 'GRADIENT', idealization: SymbolicConstantType = 'NO_IDEALIZATION', nTemp: int | None = None, thicknessModulus: float | None = None, useDensity: BooleanType = 0, density: float = 0, thicknessField: str = '', nodalThicknessField: str = '')[source]#

This method modifies the HomogeneousShellSection object.

Parameters:

thickness: A Float specifying the thickness of the section. The thickness argument applies only when *thicknessType*=UNIFORM. The default value is 0.0.
numIntPts: 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: 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: 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: 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: 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: A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.
temperature: 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: 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: 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: 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: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.
thicknessField: 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: 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.

transverseShear: TransverseShearShell = None[source]#

HomogeneousSolidSection#

class HomogeneousSolidSection(name: str, material: str, thickness: float = 1)[source]#

The HomogeneousSolidSection object defines the properties of a solid section. The HomogeneousSolidSection object is derived from the SolidSection object.

Notes

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

Methods

setValues([thickness])

This method modifies the HomogeneousSolidSection object.

setValues(thickness: float = 1)[source]#

This method modifies the HomogeneousSolidSection object.

Parameters:

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

Raises:

RangeError

LayerProperties#

class LayerProperties(barArea: float, orientationAngle: float, layerName: str, material: str, barSpacing: float = 0, layerPosition: float = 0, spacingAngle: float = 0, extensionRatio: float = 0, radius: float = 0)[source]#

The LayerProperties object defines the properties of a layer of reinforcement for membrane, shell, and surface sections.

Notes

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

LayerPropertiesArray#

class LayerPropertiesArray(iterable=(), /)[source]#

Methods

findAt

MembraneSection#

class MembraneSection(name: str, material: str, thickness: float = 1, thicknessType: SymbolicConstantType = 'UNIFORM', poissonDefinition: SymbolicConstantType = 'DEFAULT', poisson: float = 0, thicknessField: str = '')[source]#

The MembraneSection object defines the properties of a membrane section. The MembraneSection object is derived from the Section object.

Notes

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

Attributes:

rebarLayers: RebarLayers: A RebarLayers object specifying reinforcement properties.

Methods

setValues([thickness, thicknessType, ...])

This method modifies the MembraneSection object.

setValues(thickness: float = 1, thicknessType: SymbolicConstantType = 'UNIFORM', poissonDefinition: SymbolicConstantType = 'DEFAULT', poisson: float = 0, thicknessField: str = '')[source]#

This method modifies the MembraneSection object.

Parameters:

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

MPCSection#

class MPCSection(name: str, mpcType: SymbolicConstantType, userMode: SymbolicConstantType = 'DOF_MODE', userType: int = 0)[source]#

The MPCSection object defines the properties of a multi-point constraint section. The MPCSection object is derived from the Section object.

Notes

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:

PEGSection#

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

The PEGSection object defines the properties of a solid section. The PEGSection object is derived from the Section object.

Notes

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

Methods

setValues([thickness, wedgeAngle1, wedgeAngle2])

This method modifies the PEGSection object.

setValues(thickness: float = 1, wedgeAngle1: float = 0, wedgeAngle2: float = 0)[source]#

This method modifies the PEGSection object.

Parameters:

thickness: A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.
wedgeAngle1: 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: 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

RebarLayers#

class RebarLayers(rebarSpacing: SymbolicConstantType, layerTable: LayerPropertiesArray)[source]#

The RebarLayers object defines the rebar properties of a section.

Notes

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

Methods

setValues()

This method modifies the RebarLayers object.

setValues()[source]#: This method modifies the RebarLayers object.

SectionLayer#

class SectionLayer(thickness: float, material: str, orientAngle: float = 0, numIntPts: int = 3, axis: SymbolicConstantType = 'AXIS_3', angle: float = 0, additionalRotationType: SymbolicConstantType = 'ROTATION_NONE', plyName: str = '', orientation: SymbolicConstantType | None = None, additionalRotationField: str = '')[source]#

The SectionLayer object defines the material layer in a composite shell.

Notes

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

SectionLayerArray#

class SectionLayerArray(iterable=(), /)[source]#

Methods

findAt

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

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.
`MPCSection`(name, mpcType[, userMode, userType])	This method creates a MPCSection object.
`MembraneSection`(name, material[, thickness, ...])	This method creates a MembraneSection 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.

AcousticInfiniteSection(name: str, material: str, thickness: float = 1, order: int = 10) → AcousticInfiniteSection[source]#

This method creates an AcousticInfiniteSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
thickness: A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.
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. Possible values are 0 << order ≤≤ 10. The default value is 10.

Returns:

An AcousticInfiniteSection object.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

AcousticInterfaceSection(name: str, thickness: float = 1) → AcousticInterfaceSection[source]#

This method creates an AcousticInterfaceSection object.

Parameters:

name: A String specifying the repository key.
thickness: A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.

Returns:

An AcousticInterfaceSection object.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

This method creates a BeamSection object.

Parameters:

name: A String specifying the repository key.
integration: A SymbolicConstant specifying the integration method for the section. Possible values are BEFORE_ANALYSIS and DURING_ANALYSIS.
profile: A String specifying the name of the profile. This argument represents the start profile in case of *beamShape*=TAPERED.
poissonRatio: A Float specifying the Poisson’s ratio of the section. The default value is 0.0.
thermalExpansion: A Boolean specifying whether to use thermal expansion data. The default value is OFF.
temperatureDependency: A Boolean specifying whether the data depend on temperature. The default value is OFF.
dependencies: An Int specifying the number of field variable dependencies. The default value is 0.
density: None or a Float specifying the density of the section. The default value is None.
referenceTemperature: None or a Float specifying the reference temperature of the section. The default value is None.
temperatureVar: A SymbolicConstant specifying the temperature variation for the section. Possible values are LINEAR and INTERPOLATED. The default value is LINEAR.
alphaDamping: A Float specifying the αRαR factor to create mass proportional damping in direct-integration dynamics. The default value is 0.0.
betaDamping: A Float specifying the βRβR factor to create stiffness proportional damping in direct-integration dynamics. The default value is 0.0.
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). The default value is 0.0.
useFluidInertia: A Boolean specifying whether added mass effects will be simulated. The default value is OFF.
submerged: 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: 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: 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: 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: 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: 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: 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: 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: 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: A sequence of sequences of Floats specifying the items described below. The default value is an empty sequence.
outputPts: A sequence of pairs of Floats specifying the positions at which output is requested. The default value is an empty sequence.
centroid: A pair of Floats specifying the X–Y coordinates of the centroid. The default value is (0.0, 0.0).
shearCenter: A pair of Floats specifying the X–Y coordinates of the shear center. The default value is (0.0, 0.0).
profileEnd: 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.

Notes

This function can be accessed by:

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

This method creates a CohesiveSection object.

Parameters:

name: A String specifying the repository key.
response: A SymbolicConstant specifying the geometric assumption that defines the constitutive behavior of the cohesive elements. Possible values are TRACTION_SEPARATION, CONTINUUM, and GASKET.
material: A String specifying the name of the material.
initialThicknessType: 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: A Float specifying the initial thickness for the section. The initialThickness argument applies only when *initialThicknessType*=SPECIFY. The default value is 1.0.
outOfPlaneThickness: None or a Float specifying the out-of-plane thickness for the section. The default value is None.

Returns:

A CohesiveSection object.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

This method creates a CompositeShellSection object.

Parameters:

name: A String specifying the repository key.
layup: A SectionLayerArray object specifying the shell cross-section.
symmetric: A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.
thicknessType: 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: 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: 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: 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: A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.
temperature: 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: 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: 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: 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: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.
layupName: A String specifying the layup name for this section. The default value is an empty string.
thicknessField: 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: 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.

Notes

This function can be accessed by:

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

CompositeSolidSection(name: str, layup: SectionLayerArray, symmetric: BooleanType = 0, layupName: str = '') → CompositeSolidSection[source]#

This method creates a CompositeSolidSection object.

Parameters:

name: A String specifying the repository key.
layup: A SectionLayerArray object specifying the solid cross-section.
symmetric: A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.
layupName: A String specifying the layup name for this section. The default value is an empty string.

Returns:

A CompositeSolidSection object.

Notes

This function can be accessed by:

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

This method creates a ConnectorSection object.

Parameters:

name: A String specifying the repository key.
assembledType: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: 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: A ConnectorBehaviorOptionArray object.

Returns:

A ConnectorSection object.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

EulerianSection(name: str, data: str) → EulerianSection[source]#

This method creates a EulerianSection object.

Parameters:

name: A String specifying the repository key.
data: 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.

Notes

This function can be accessed by:

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

This method creates a GasketSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material of which the gasket is made or material that defines gasket behavior.
crossSection: 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: A Float specifying the initial gap. The default value is 0.0.
initialThickness: 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: A Float specifying the initial void. The default value is 0.0.
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. 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.

Notes

This function can be accessed by:

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

This method creates a GeneralStiffnessSection object.

Parameters:

name: A String specifying the repository key.
stiffnessMatrix: 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: None or a Float specifying the reference temperature for thermal expansion. The default value is None.
applyThermalStress: A Boolean specifying whether or not the section stiffness varies with thermal stresses. The default value is OFF.
temperatureDependency: A Boolean specifying whether the data depend on temperature. The default value is OFF.
dependencies: An Int specifying the number of field variable dependencies. The default value is 0.
poissonDefinition: 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: 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: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.
thermalStresses: 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: 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.

Notes

This function can be accessed by:

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

This method creates a HomogeneousShellSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the section material.
thickness: A Float specifying the thickness of the section. The thickness argument applies only when *thicknessType*=UNIFORM. The default value is 0.0.
numIntPts: 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: 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: 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: 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: 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: A SymbolicConstant specifying the shell section integration rule. Possible values are SIMPSON and GAUSS. The default value is SIMPSON.
temperature: 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: 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: 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: 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: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.
thicknessField: 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: 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.

Notes

This function can be accessed by:

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

HomogeneousSolidSection(name: str, material: str, thickness: float = 1) → HomogeneousSolidSection[source]#

This method creates a HomogeneousSolidSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
thickness: A Float specifying the thickness of the section. Possible values are None or greater than zero. The default value is 1.0.

Returns:

A HomogeneousSolidSection object.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

MPCSection(name: str, mpcType: SymbolicConstantType, userMode: SymbolicConstantType = 'DOF_MODE', userType: int = 0) → MPCSection[source]#

This method creates a MPCSection object.

Parameters:

name: A String specifying the repository key.
mpcType: 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: 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: 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.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

This method creates a MembraneSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
thickness: A Float specifying the thickness for the section. Possible values are thickness >> 0.0. The default value is 1.0.
thicknessType: 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: 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: 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: 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.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

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

This method creates a PEGSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
thickness: A Float specifying the thickness of the section. Possible values are thickness >> 0.0. The default value is 1.0.
wedgeAngle1: 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: 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.

Raises:

InvalidNameError
RangeError

Notes

This function can be accessed by:

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

SurfaceSection(name: str, useDensity: BooleanType = 0, density: float = 0) → SurfaceSection[source]#

This method creates a SurfaceSection object.

Parameters:

name: A String specifying the repository key.
useDensity: A Boolean specifying whether or not to use the value of density. The default value is OFF.
density: A Float specifying the value of density to apply to this section. The default value is 0.0.

Returns:

A SurfaceSection object.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

TrussSection(name: str, material: str, area: float = 1) → TrussSection[source]#

This method creates a TrussSection object.

Parameters:

name: A String specifying the repository key.
material: A String specifying the name of the material.
area: 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.

Raises:

RangeError and InvalidNameError.

Notes

This function can be accessed by:

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

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.

Notes

This object can be accessed by:

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

Attributes:

name: str: A String specifying the repository key.
transverseShear: TransverseShearShell: A TransverseShearShell object specifying the transverse shear stiffness properties.

transverseShear: TransverseShearShell = None[source]#

SolidSection#

class SolidSection[source]#

Notes

This object can be accessed by:

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

Attributes:

name: str: A String specifying the repository key.

SurfaceSection#

class SurfaceSection(name: str, useDensity: BooleanType = 0, density: float = 0)[source]#

The SurfaceSection object defines the properties of a surface section. The SurfaceSection object is derived from the Section object.

Notes

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

Attributes:

rebarLayers: RebarLayers: A RebarLayers object specifying reinforcement properties.

TransverseShearBeam#

class TransverseShearBeam(scfDefinition: SymbolicConstantType, k23: float | None = None, k13: float | None = None, slendernessCompensation: SymbolicConstantType | float = 0)[source]#

The TransverseShearBeam object defines the transverse shear stiffness properties of a beam section.

Notes

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

Methods

setValues()

This method modifies the TransverseShearBeam object.

setValues()[source]#: This method modifies the TransverseShearBeam object.

TransverseShearShell#

class TransverseShearShell(k11: float, k22: float, k12: float)[source]#

The TransverseShearShell object defines the transverse shear stiffness properties of a shell section.

Notes

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

Methods

setValues()

This method modifies the TransverseShearShell object.

setValues()[source]#: This method modifies the TransverseShearShell object.

TrussSection#

class TrussSection(name: str, material: str, area: float = 1)[source]#

The TrussSection object defines the properties of a truss section. The TrussSection object is derived from the Section object.

Notes

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

Methods

setValues([area])

This method modifies the TrussSection object.

setValues(area: float = 1)[source]#

This method modifies the TrussSection object.

Parameters:

area: A Float specifying the cross-sectional area for the section. Possible values are area >> 0. The default value is 1.0.

Raises:

RangeError