Part

Features in Abaqus/CAE include Parts, Datums, Partitions, and Assembly operations. Part commands create Feature objects on only the Part object. The commands that create Feature objects on only the rootAssembly object are described in Assembly commands. The commands that create Feature objects on both the Part and the rootAssembly objects are described in Feature commands.

Create parts

class PartModel(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)

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

Notes

This object can be accessed by:

mdb.models[name]

Methods

Part(name, dimensionality, type[, twist])

This method creates a Part object and places it in the parts repository.

Part(name: str, dimensionality: SymbolicConstantType, type: SymbolicConstantType, twist: BooleanType = 0)

This method creates a Part object and places it in the parts repository.

Parameters:

name

A String specifying the repository key.

dimensionality

A SymbolicConstant specifying the dimensionality of the part. Possible values are THREE_D, TWO_D_PLANAR, and AXISYMMETRIC.

type

A SymbolicConstant specifying the type of the part. Possible values are DEFORMABLE_BODY, EULERIAN, DISCRETE_RIGID_SURFACE, and ANALYTIC_RIGID_SURFACE.

twist

A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when *dimensionality*=AXISYMMETRIC and *type*=DEFORMABLE_BODY). The default value is OFF.

Returns:

A Part object.

Notes

This function can be accessed by:

mdb.models[name].Part

class PartBase(name: str, dimensionality: SymbolicConstantType, type: SymbolicConstantType, twist: BooleanType = OFF)

class PartBase(name: str, objectToCopy: str, scale: float = 1, mirrorPlane: SymbolicConstantType = NONE, compressFeatureList: BooleanType = OFF, separate: BooleanType = OFF)

The Part object defines the physical attributes of a structure. Parts are instanced into the assembly and positioned before an analysis.

Notes

This object can be accessed by:

import part
mdb.models[name].parts[name]

Attributes:

geometryValidity: Boolean

A Boolean specifying the validity of the geometry of the part. The value is computed, but it can be set to ON to perform feature and mesh operations on an invalid part. There is no guarantee that such operations will work if the part was originally invalid.

isOutOfDate: int

An Int specifying that feature parameters have been modified but that the part has not been regenerated. Possible values are 0 and 1.

timeStamp: float

A Float specifying when the part was last modified.

vertices: VertexArray

A VertexArray object specifying all the vertices in the part.

ignoredVertices: IgnoredVertexArray

An IgnoredVertexArray object specifying all the ignored vertices in the part.

edges: EdgeArray

An EdgeArray object specifying all the edges in the part.

ignoredEdges: IgnoredEdgeArray

An IgnoredEdgeArray object specifying all the ignored edges in the part.

faces: FaceArray

A FaceArray object specifying all the faces in the part.

cells: CellArray

A CellArray object specifying all the cells in the part.

features: dict[str, Feature]

A repository of Feature objects specifying all the features in the part.

featuresById: dict[str, Feature]

A repository of Feature objects specifying all Feature objects in the part. The Feature objects in the featuresById repository are the same as the Feature objects in the features’ repository. However, the key to the objects in the featuresById repository is an integer specifying the ID, whereas the key to the objects in the features’ repository is a string specifying the name. datums: list[Datum] A repository of Datum objects specifying all the datums in the part.

elements: MeshElementArray

A MeshElementArray object specifying all the elements in the part.

elemFaces: dict[str, MeshFace]

A repository of MeshFace objects specifying all the element faces in the part. For a given element and a given face index within that element, the corresponding MeshFace object can be retrieved from the repository by using the key calculated as (i*8 + j), where i and j are zero-based element and face indices, respectively.

elementFaces: MeshFaceArray

A MeshFaceArray object specifying all the unique element faces in the part.

nodes: MeshNodeArray

A MeshNodeArray object specifying all the nodes in the part.

retainedNodes: MeshNodeArray

A MeshNodeArray object specifying all the retained nodes in the substructure part.

sets: dict[str, Set]

A repository of Set objects specifying for more information, see Set.

allSets: dict[str, Set]

A repository of Set objects specifying the contents of the all :py:class:`~abaqus.Region.Set.Set`s repository is the same as the contents of the sets repository.

allInternalSets: dict[str, Set]

A repository of Set objects specifying picked regions.

surfaces: dict[str, Surface]

A repository of Surface objects specifying for more information, see Surface.

allSurfaces: dict[str, Surface]

A repository of Surface objects specifying the contents of the allSurfaces repository is the same as the contents of the surfaces repository.

allInternalSurfaces: dict[str, Surface]

A repository of Surface objects specifying picked regions.

skins: dict[str, Skin]

A repository of Skin objects specifying the skins created on the part.

stringers: dict[str, Stringer]

A repository of Stringer objects specifying the stringers created on the part.

referencePoints: ReferencePoints

A repository of ReferencePoint objects.

engineeringFeatures: EngineeringFeature

An EngineeringFeature object.

sectionAssignments: SectionAssignmentArray

A SectionAssignmentArray object.

materialOrientations: MaterialOrientationArray

A MaterialOrientationArray object.

compositeLayups: dict[str, CompositeLayup]

A repository of CompositeLayup objects.

elemEdges: dict[str, MeshEdge]

A repository of MeshEdge. MeshEdge` objects specifying all the element edges in the part. For a given element and a given edge index on a given face within that element, the corresponding MeshEdge. MeshEdge` object can be retrieved from the repository by using the key calculated as (i*32 + j*4 + k), where i, j, and k are zero-based element, face, and edge indices, respectively.

elementEdges: MeshEdgeArray

A MeshEdgeArray object specifying all the unique element edges in the part.

Methods

Lock()	This method locks the part.
LockForUpgrade()	This method locks the part for upgrade.
Part2DGeomFrom2DMesh(name, part, featureAngle)	This method creates a geometric Part object from the outline of an existing two-dimensional orphan mesh Part object and places it in the parts repository.
PartFromBooleanCut(name, instanceToBeCut, ...)	This method creates a Part in the parts repository after subtracting or cutting the geometries of a group of part instances from that of a base part instance.
PartFromBooleanMerge(name, instances[, ...])	This method creates a Part in the parts repository after merging two or more part instances.
PartFromExtrude2DMesh(name, part, depth, ...)	This method creates a Part object by extruding an existing two-dimensional orphan mesh Part object in the positive Z-direction and places it in the parts repository.
PartFromGeometryFile(name, geometryFile, ...)	This method creates a Part object and places it in the parts repository.
PartFromInstanceMesh(name[, partInstances, ...])	This method creates a Part object containing the mesh found in the supplied PartInstance objects and places the new Part object in the parts repository.
PartFromMesh(name[, copySets])	This method creates a Part object containing the mesh found in the part and places the new Part object in the parts repository.
PartFromMeshMirror(name, part, point1, point2)	This method creates a Part object by mirroring an existing orphan mesh Part object about a specified plane and places it in the parts repository.
PartFromNodesAndElements(name, ...[, twist])	This method creates a Part object from nodes and elements and places it in the parts repository.
PartFromOdb(name, odb[, fileName, instance, ...])	This method creates an orphan mesh Part object by reading an output database.
PartFromSection3DMeshByPlane(name, part, ...)	This method creates a Part object by cutting an existing three-dimensional orphan mesh Part object by a plane and places it in the parts repository.
PartFromSubstructure(name, substructureFile, ...)	This method creates a substructure Part object by reading a substructure sim file and places it in the parts repository.
Unlock()	This method unlocks the part.
addGeomToSketch(sketch)	This method converts a part into a sketch by projecting all of the edges of the part onto the X-Y plane of the sketch.
assignThickness(faces[, thickness, ...])	This method assigns thickness data to shell faces.
backup()	This method makes a backup copy of the features in the part.
checkGeometry([detailed, reportFacetErrors, ...])	This method checks the validity of the geometry of the part and prints a count of all topological entities on the part (faces, edges, vertices, etc.).
clearGeometryCache()	This method clears the geometry cache.
copyMeshPattern([elements, faces, ...])	This method copies a mesh pattern from a source region consisting of a set of shell elements or element faces onto a target face, mapping nodes and elements in a one-one correspondence between source and target.
deleteAllFeatures()	This method deletes all the features in the part.
deleteFeatures(featureNames)	This method deletes the given features.
getAngle(plane1, plane2, line1, line2[, ...])	This method returns the angle between the specified entities.
getArea(faces[, relativeAccuracy])	This method returns the total surface area of a given face or group of faces.
getAssociatedCADPaths()	This method returns the paths to the associated CAD part and root file.
getCADParameters()	This method returns the names and values of the CAD parameters associated with the part.
getCentroid(faces, cells[, relativeAccuracy])	Depending on the arguments provided, this method returns the following:
getCoordinates(entity, csys)	This method returns the coordinates of specified point.
getCurvature(edges[, samplePoints])	This method returns the maximum curvature of a given edge or group of edges.
getDistance(entity1, entity2)	Depending on the arguments provided, this method returns one of the following:
getFeatureCells(name)	This method returns a sequence of Cell objects that are created by the given feature.
getFeatureEdges(name)	This method returns a sequence of Edge objects that are created by the given feature.
getFeatureFaces(name)	This method returns a sequence of Face objects that are created by the given feature.
getFeatureVertices(name)	This method returns a sequence of ConstrainedSketchVertex objects that are created by the given feature.
getLength(edges)	This method returns the length of a given edge or group of edges.
getMassProperties([regions, ...])	This method returns the mass properties of a part or region.
getPerimeter(faces)	This method returns the total perimeter of a given face or group of faces.
getVolume(cells[, relativeAccuracy])	This method returns the volume area of a given cell or group of cells.
isAlignedWithSketch()	This method checks if the normal of an analytical rigid surface part is aligned with that of its sketch.
printAssignedSections()	This method prints information on each section that has been assigned to a region of the part.
projectEdgesOntoSketch(sketch, edges[, ...])	This method projects the selected edges of a part onto the specified ConstrainedSketch object.
projectReferencesOntoSketch(sketch[, ...])	This method projects the vertices of specified edges, and datum points from the part onto the specified ConstrainedSketch object.
queryAttributes([printResults])	This method prints the following information about a part:
queryCachedStates()	This method displays the position of geometric states relative to the sequence of features in the part cache.
queryDisjointPlyRegions()	This method provides a list of all composite plys in the current part which have disjoint regions.
queryGeometry([relativeAccuracy, printResults])	This method prints the following information about a part:
queryRegionsMissingSections()	This method returns all regions in the part that do not have a section assignment but require one for analysis.
regenerate()	This method regenerates a part.
regenerationWarnings()	This method prints any regeneration warnings associated with the features.
removeInvalidGeometry()	Removes all invalid entities from the part, leaving a valid part.
restore()	This method restores the parameters of all features in the assembly to the value they had before a failed regeneration.
resumeAllFeatures()	This method resumes all the suppressed features in the part.
resumeFeatures(featureNames)	This method resumes the specified suppressed features in the part.
resumeLastSetFeatures()	This method resumes the last set of features to be suppressed in the part.
saveGeometryCache()	This method caches the current geometry.
setAssociatedCADPaths([partFile, rootFile])	This method sets the paths to the associated CAD part and root file.
setValues(*args, **kwargs)	This method modifies the Part object.
smoothNodes(nodes)	This method smooths the given nodes of a native mesh, moving them locally to a more optimal location that improves the quality of the mesh
suppressFeatures(featureNames)	This method suppresses the given features.
writeAcisFile(fileName[, version])	This method exports the geometry of the part to a named file in ACIS format.
writeCADParameters(paramFile[, ...])	This method writes the parameters that were imported from the CAD system to a parameter file.
writeIgesFile(fileName, flavor)	This method exports the geometry of the part to a named file in IGES format.
writeStepFile(fileName)	This method exports the geometry of the part to a named file in STEP format.
writeVdaFile(fileName)	This method exports the geometry of the part to a named file in VDA-FS format.

Lock()

This method locks the part. Locking the part prevents any further changes to the part that can trigger regeneration of the part.

LockForUpgrade()

This method locks the part for upgrade. Locking the part prevents any further changes to the part that can trigger regeneration of the part. When the part is unlocked, all the parts are upgraded and regenrated.

Part2DGeomFrom2DMesh(name: str, part: PartBase, featureAngle: float, splineCurvatureLimit: float = 90, twist: BooleanType = 0)

This method creates a geometric Part object from the outline of an existing two-dimensional orphan mesh Part object and places it in the parts repository. If the Part2DGeomFrom2DMesh method cannot create a valid two-dimensional shell section from the two-dimensional mesh, the method fails and creates an empty geometry part with a failed base shell feature.

Parameters:

name

A String specifying the repository key.

part

A Part object specifying an existing two-dimensional orphan mesh Part object.

featureAngle

A Float specifying the angle (in degrees) between line segments that triggers a break in the geometry.

splineCurvatureLimit

A Float specifying the traversal angle in degrees of the spline that triggers a break in the geometry. The default value is 90.

twist

A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when *dimensionality*=AXISYMMETRIC and *type*=DEFORMABLE_BODY). The default value is OFF.

Returns:

part: Part

A Part object If the specified part is not an orphan mesh part:

Specified part must be an orphan mesh.

If the Part2DGeomFrom2DMesh method cannot create a valid two-dimensional shell section from the two-dimensional mesh:

Planar shell feature failed

If the specified part is not two-dimensional:

Cannot create a geometry from a 3D part.

If the specified part is a rigid body:

Cannot create a geometry from a rigid body.

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromBooleanCut(name: str, instanceToBeCut: str, cuttingInstances: tuple[abaqus.Part.PartBase.PartInstance])

This method creates a Part in the parts repository after subtracting or cutting the geometries of a group of part instances from that of a base part instance.

Parameters:

name

A String specifying the repository key.

instanceToBeCut

A PartInstance specifying the base instance from which to cut other instances.

cuttingInstances

A sequence of PartInstance objects specifying the instances with which to cut the base instance.

Returns:

part: Part

A Part object

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromBooleanMerge(name: str, instances: tuple[abaqus.Part.PartBase.PartInstance], keepIntersections: BooleanType = False, mergeNodes: SymbolicConstantType = 'BOUNDARY_ONLY', nodeMergingTolerance: float | None = None, removeDuplicateElements: BooleanType = 1, domain: SymbolicConstantType = 'GEOMETRY')

This method creates a Part in the parts repository after merging two or more part instances. The part instances can be either Abaqus native parts or orphan mesh parts, but they cannot be a combination of both.

Parameters:

name

A String specifying the repository key.

instances

A sequence of PartInstance objects specifying the part instances to merge.

keepIntersections

A Boolean specifying whether the boundary intersections of Abaqus native part instances should be retained after the merge operation. The default value is False.

mergeNodes

A SymbolicConstant specifying whether the nodes of orphan mesh part instances should be retained after the merge operation. Possible values are BOUNDARY_ONLY, ALL, or NONE. The default value is BOUNDARY_ONLY.

nodeMergingTolerance

A Float specifying the maximum distance between nodes of orphan mesh part instances that will be merged and replaced with a single new node. The location of the new node is the average position of the deleted nodes. The default value is 10–6.

removeDuplicateElements

A Boolean specifying whether elements with the same connectivity after the merge will merged into a single element. The default value is ON.

domain

A SymbolicConstant specifying whether the part instances being merged are geometric instances or mesh instances. Possible values are GEOMETRY, MESH or BOTH. The default value is GEOMETRY.

Returns:

part: Part

A Part object

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromExtrude2DMesh(name: str, part: PartBase, depth: float, elementSize: float)

This method creates a Part object by extruding an existing two-dimensional orphan mesh Part object in the positive Z-direction and places it in the parts repository.

Parameters:

name

A String specifying the repository key.

part

A Part object specifying an existing two-dimensional orphan mesh Part object.

depth

A Float specifying the total extrusion distance.

elementSize

A Float specifying an approximate element length in the extruded direction.

Returns:

part: Part

A Part object - If the specified part is not an orphan mesh part:

Cannot extrude a geometric part.

• If the specified part is not two-dimensional: Cannot extrude a 3D part.

• If the specified part is a rigid body: Cannot change dimension of a rigid body.

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromGeometryFile(name: str, geometryFile: AcisFile, dimensionality: SymbolicConstantType, type: SymbolicConstantType, bodyNum: int = 1, combine: BooleanType = False, booleanSolids: BooleanType = False, retainBoundary: BooleanType = False, usePartNameFromFile: BooleanType = 0, stitchTolerance: float = 1, twist: BooleanType = 0, scale: float = 1, convertToAnalytical: int = 0, convertToPrecise: int = 0)

This method creates a Part object and places it in the parts repository.

Parameters:

name

A String specifying the repository key.

geometryFile

An AcisFile object specifying a file containing geometry.

dimensionality

A SymbolicConstant specifying the dimensionality of the part. Possible values are THREE_D, TWO_D_PLANAR, and AXISYMMETRIC.

type

A SymbolicConstant specifying the type of the part. Possible values are DEFORMABLE_BODY, EULERIAN, DISCRETE_RIGID_SURFACE, and ANALYTIC_RIGID_SURFACE.

bodyNum

An Int specifying the desired body to be selected from an ACIS object containing a list of N ACIS bodies. Possible values are 1 ≤≤ bodyNum ≤≤ N. The default value is 1.

combine

A Boolean specifying weather to create a single part by combining all the bodies in the ACIS object. This argument is ignored if bodyNum is specified. The default value is False.

booleanSolids

A Boolean specifying whether the solids should be boolean while combining all the bodies.The default value is FALSE.

retainBoundary

A Boolean specifying whether the intersecting boundaries should be retained while boolean the solids.The default value is FALSE.

usePartNameFromFile

A Boolean specifying whether the part names specified in a STEP file should be used as the names in the Abaqus model database. If this option is TRUE, the part names in the STEP file will be used; if FALSE, each imported part will be named using the text of the name argument followed by a number. This functionality is available only for import from STEP files; for import from all other types of files this option should be FALSE.

stitchTolerance

A Float indicating the maximum gap to be stitched. The value should be smaller than the minimum feature size and bigger than the maximum gap expected to be stitched in the model. Otherwise this command may remove small (sliver) edges that are smaller than the tolerance. The default value is 1.0

twist

A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when *dimensionality*=AXISYMMETRIC and *type*=DEFORMABLE_BODY). The default value is OFF.

scale

A Float specifying the scaling factor to apply to the imported geometric entities. The default value is 1.0.

convertToAnalytical

An Int specifying whether to convert to analytical entities. Possible values are 0 or 1. The default value is 0. If *convertToAnalytical*=1, all the numerical entities, such as splines, are converted to analytical entities, such as arcs and lines, during the repair phase of the command.

convertToPrecise

An Int specifying whether to convert to precise geometry. Possible value are 0 or 1. The default value is 0. If *convertToPrecise*=1, the application will attempt to re-evaluate the tolerant entities to be more precise.

Returns:

part: Part

A Part object - If the ACIS file is corrupt:

PartError: the file is corrupt

• If the dimensionality does not correspond to what is found in the ACIS file: PartError: dimensionality does not match the contents of the file

• If the type does not correspond to what is found in the ACIS file: PartError: type does not match the contents of the file

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromInstanceMesh(name: str, partInstances: tuple[abaqus.Part.PartBase.PartInstance] = (), copyPartSets: BooleanType = False, copyAssemblySets: BooleanType = False)

This method creates a Part object containing the mesh found in the supplied PartInstance objects and places the new Part object in the parts repository.

Parameters:

name

A String specifying the repository key.

partInstances

A sequence of PartInstance objects to be used in the creation of the new mesh part. If the partInstances argument is omitted, the new Part object contains the mesh of all the part instances in the assembly.

copyPartSets

A Boolean specifying whether to copy sets, surfaces, and attributes from the base part or parts of the specified part instances to the new part. The default is False.

copyAssemblySets

A Boolean specifying whether to copy assembly-level sets that reference entities of the specified part instances to the new part. The default is False.

Returns:

part: Part

A Part object - If the analysis type (deformable or rigid) is not consistent among the supplied part instances:

The selected part instances do not have a consistent analysis type.

• If the assembly does not contain a mesh: The current assembly does not contain a mesh for a mesh part.

• If the specified part instances do not contain a mesh: The selected part instances do not have a mesh for a mesh part.

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromMesh(name: str, copySets: BooleanType = False)

This method creates a Part object containing the mesh found in the part and places the new Part object in the parts repository.

Parameters:

name

A String specifying the repository key.

copySets

A Boolean specifying whether to copy sets, surfaces, and attributes to the new part. The default is False.

Returns:

part: Part

A Part object - If the part does not contain a mesh:

The current part does not contain a mesh for a mesh part.

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromMeshMirror(name: str, part: PartBase, point1: tuple, point2: tuple)

This method creates a Part object by mirroring an existing orphan mesh Part object about a specified plane and places it in the parts repository. The result is a union of the original and the mirrored copy. Contrast the PartFromMeshMirror method with the mirrorPlane argument of the Part copy constructor. The mirrorPlane argument creates only the second half of the part but does not unite the two halves.

Parameters:

name

A String specifying the repository key.

part

A Part object specifying an existing orphan mesh part.

point1

A sequence of three Floats specifying a point on the mirror plane. This point is the local origin in the local system of the plane.

point2

A sequence of three Floats specifying a point in the direction of the normal to the mirror plane. This point must not be coincident with point1.

Returns:

part: Part

A Part object - If the specified part is not an orphan mesh part:

Cannot mirror a geometric part.

• If the specified part is a rigid body: Cannot mirror a rigid body.

• If point1 and point2 are coincident: Mirror plane director has zero length.

• If the specified part is two-dimensional and the plane is not parallel to the

Z-axis:

Mirror plane must be parallel to Z axis for 2D parts

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromNodesAndElements(name: str, dimensionality: SymbolicConstantType, type: SymbolicConstantType, nodes: tuple, elements: tuple, twist: BooleanType = 0)

This method creates a Part object from nodes and elements and places it in the parts repository.

Parameters:

name

A String specifying the repository key.

dimensionality

A SymbolicConstant specifying the dimensionality of the part. Possible values are THREE_D, TWO_D_PLANAR, and AXISYMMETRIC.

type

A SymbolicConstant specifying the type of the part. Possible values are DEFORMABLE_BODY, EULERIAN, DISCRETE_RIGID_SURFACE, and ANALYTIC_RIGID_SURFACE.

nodes

A sequence of (nodeLabels, nodeCoords) specifying the nodes of the mesh. nodeLabels is a sequence of Ints specifying the node labels, and nodeCoords is a sequence of sequences of three Floats specifying the nodal coordinates.

elements

A sequence of sequences of(meshType, elementLabels, elementConns) specifying the elements of the mesh. meshType is a String specifying the element type. elementlabels is a sequence of Ints specifying the element labels. elementConns is a sequence of sequences of node labels specifying the element connectivity.

twist

A boolean specifying whether the part is defined with twist. This option has meaning only when *dimensionality*=AXISYMMETRIC. Possible values are ON and OFF. The default value is OFF.

Returns:

part: Part

A Part object

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromOdb(name: str, odb: str, fileName: str = '', instance: str = '', elementSet: str = '', shape: SymbolicConstantType = 'UNDEFORMED', step: int | None = None, frame: int | None = None, twist: BooleanType = 0)

This method creates an orphan mesh Part object by reading an output database. The new part is placed in the parts repository.

Parameters:

name

A String specifying the repository key.

odb

An output database object.

fileName

A String specifying the name of the output database file from which to create the part. The default value is an empty string.

instance

A String specifying the part instance in the output database from which to create the part. If no instance name is specified, Abaqus creates an orphan mesh part from the first part instance in the output database.

elementSet

A String specifying an element set defined on the output database. Only elements from this set will be imported. The default is to import all element sets.

shape

A SymbolicConstant specifying the configuration state. Possible values are UNDEFORMED and DEFORMED. The default value is UNDEFORMED.

step

An Int specifying the step number for reading deformed coordinates. 0≤step≤N−10≤step≤N-1 where NN is the number of available steps. The default value is the last available step. You should specify the step argument only when *shape*=DEFORMED.

frame

An Int specifying the frame number for reading deformed coordinates. 0≤frame≤N−10≤frame≤N-1 where NN is the number of available frames. The default value is the last available frame. You should specify the frame argument only when *shape*=DEFORMED.

twist

A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when *dimensionality*=AXISYMMETRIC and *type*=DEFORMABLE_BODY). The default value is OFF.

Returns:

part: Part

A Part object - If the output database contains elements of more than one dimensionality or type:

File contains both axisymmetric and nonaxisymmetric elements.File contains both 2D and

3D elements.File contains both rigid and deformable elements. - If more than one part is found on the output database:

PartError: importing of more than one part is not currently supported

• If the output database does not contain any valid results for the specified step: Error. File does not contain any valid frames.

• If the specified step and frame do not contain any displacements: Error. Specified frame does not contain nodal displacements.

• If the specified element set is not found on the output database: Error. Specified element set is not defined in the ODB.

• If the step number is invalid: OdiError: Invalid step index: i. Available step indices: 0 - j.

• If the frame number is invalid: OdiError: Invalid frame index: i. Available frame indices: 0 - j.

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromSection3DMeshByPlane(name: str, part: PartBase, point1: float, point2: float, point3: tuple)

This method creates a Part object by cutting an existing three-dimensional orphan mesh Part object by a plane and places it in the parts repository. This method is valid only for orphan mesh parts composed of 8-node brick elements.

Parameters:

name

A String specifying the repository key.

part

A Part object specifying an existing three-dimensional orphan mesh part.

point1

A Sequence of three Floats specifying a point on the cutting plane. This point is the local origin in the local system of the plane.

point2

A Sequence of three Floats specifying a point in the direction of the normal to the cutting plane. This point must not be coincident with point1.

point3

A sequence of three Floats specifying the direction of the local 1-axis in the local system of the plane. This point must not project onto point1.

Returns:

part: Part

A Part object - If the specified part is not an orphan mesh part:

Cannot reduce dimension of a geometric part.

• If the specified part is not three-dimensional: Cannot reduce dimension of a 2D part.

• If the specified part is a rigid body: Cannot change dimension of a rigid body.

• If point1 and point2 are coincident: Cutting plane director has zero length.

• If point3 projects onto point1: Local axis point projects to origin.

• If no elements are cut by the specified plane: Cannot reduce part dimension.

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromSubstructure(name: str, substructureFile: str, odbFile: str)

This method creates a substructure Part object by reading a substructure sim file and places it in the parts repository.

Parameters:

name

A String specifying the repository key.

substructureFile

A substructure sim file.

odbFile

The output database file corresponding to the substructure sim file.

Returns:

part: Part

A Part object - If the specified part is not a substructure:

File specified does not contain a substructure.

• If the specified part already exists: A part with the same name already exists.

• If the substructure cannot be imported: The output database is missing nodes and elements.Nested substructures are not

supported.The substructure sim file was generated using a version that is different from the current version.

Notes

This function can be accessed by:

mdb.models[name].Part

Unlock()

This method unlocks the part. Unlocking the part allows it to be regenerated after any modifications to the part.

addGeomToSketch(sketch: ConstrainedSketch)

This method converts a part into a sketch by projecting all of the edges of the part onto the X-Y plane of the sketch. You can use addGeomToSketch with a part of any modeling space.

Parameters:

sketch

A ConstrainedSketch object.

assignThickness(faces: tuple[Face], thickness: float | None = None, topFaces: tuple[Face] = (), bottomFaces: tuple[Face] = ())

This method assigns thickness data to shell faces. The thickness can be used while assigning shell and membrane sections to faces.

Parameters:

faces

A sequence of Face objects specifying the regions where thickness will be applied.

thickness

A Float specifying the thickness along the given faces . Either thickness, topFaces, or bottomFaces must be specified.

topFaces

A sequence of Face objects whose distance to faces argument is used to calculate the thickness along the faces. The combination of topFaces and bottomFaces determines the thickness and the offset of the elements. If bottomFaces is not specified then the thickness is twice the distance to the topFaces. This argument will be ignored if thickness is specified. Either thickness, topFaces, or bottomFaces must be specified.

bottomFaces

A sequence of Face objects whose distance to faces is used to calculate the thickness along the faces. The combination of topFaces and bottomFaces determines the thickness and the offset of the elements. If topFaces is not specified then the thickness is twice the distance to the bottomFaces. This argument will be ignored if thickness is specified. Either thickness, topFaces, or bottomFaces must be specified.

backup()

This method makes a backup copy of the features in the part. Use the restore method to retrieve the part’s features from the backup.

checkGeometry(detailed: BooleanType = 0, reportFacetErrors: BooleanType = 0, level: int | None = None)

This method checks the validity of the geometry of the part and prints a count of all topological entities on the part (faces, edges, vertices, etc.).

Parameters:

detailed

A Boolean specifying whether detailed output will be printed to the replay file. The default value is OFF.

reportFacetErrors

A Boolean specifying whether faces are checked for proper facetting. The default value is OFF.

level

An Int specifying which level of checking is performed. Values can range from 20 to 70, with higher values reporting less and less important errors. The default value is 20, which reports all critical errors. When the default value is used, the stored validity status is updated to agree with the result of this check.

clearGeometryCache()

This method clears the geometry cache. Clearing the geometry cache reduces the amount of memory being used to cache part features.

copyMeshPattern(elements: tuple[abaqus.Mesh.MeshElement.MeshElement] = (), faces: tuple[abaqus.BasicGeometry.Face.Face] = (), elemFaces: tuple[abaqus.Mesh.MeshFace.MeshFace] = (), targetFace: ~abaqus.Mesh.MeshFace.MeshFace = <abaqus.Mesh.MeshFace.MeshFace object>, nodes: tuple[abaqus.Mesh.MeshNode.MeshNode] = (), coordinates: tuple = ())

This method copies a mesh pattern from a source region consisting of a set of shell elements or element faces onto a target face, mapping nodes and elements in a one-one correspondence between source and target.

Parameters:

elements

A sequence of MeshElement objects or a Set object containing elements and specifying the source region.

faces

A sequence of Face objects that have associated with shell elements or element faces and specifying the source region.

elemFaces

A sequence of MeshFace objects specifying the source region.

targetFace

A MeshFace object specifying the target region.

nodes

A sequence of MeshNode objects or a Set object containing nodes on the boundary of source region which are to be positioned to the boundary of target face.

coordinates

A sequence of three-dimensional coordinate tuples specifying the coordinates for each of the given nodes. When specified, the number of coordinate tuples must match the number of given nodes, and be ordered to correspond to the given nodes in ascending order according to index. These coordinates are positions of the nodes of a mesh that will be the target face corresponding to nodes provided.

deleteAllFeatures()

This method deletes all the features in the part.

deleteFeatures(featureNames: tuple)

This method deletes the given features.

Parameters:

featureNames

A sequence of Strings specifying the feature names that will be deleted from the part.

getAngle(plane1: str, plane2: str, line1: str, line2: str, commonVertex: str = '')

This method returns the angle between the specified entities.

Parameters:

plane1

A Face, MeshFace, or a Datum object specifying the first plane. The Datum object must represent a datum plane. The plane1 and line1 arguments are mutually exclusive. One of them must be specified.

plane2

A Face, MeshFace, or a Datum object specifying the second plane. The Datum object must represent a datum plane. The plane2 and line2 arguments are mutually exclusive. One of them must be specified.

line1

An Edge, MeshEdge, or a Datum object specifying the first curve. The Datum object must represent a datum axis. The plane1 and line1 arguments are mutually exclusive. One of them must be specified.

line2

An Edge, MeshEdge, or a Datum object specifying the second curve. The Datum object must represent a datum axis. The plane2 and line2 arguments are mutually exclusive. One of them must be specified.

commonVertex

If the two selected Edge objects have more than one vertex in common, this ConstrainedSketchVertex object specifies the vertex at which to evaluate the angle.

Returns:

angle: python:float

A Float specifying the angle between the specified entities. If you provide a plane as an argument, Abaqus/CAE computes the angle using the normal to the plane.

getArea(faces: tuple[Face], relativeAccuracy: float = 0)

This method returns the total surface area of a given face or group of faces.

Parameters:

faces

A sequence of Face objects whose area the method will calculate.

relativeAccuracy

A Float specifying that the area computation should stop when the specified relative accuracy has been achieved. The default value is 0.000001 (0.0001%).

Returns:

area: python:float

A Float specifying the sum of the calculated areas of the given faces.

getAssociatedCADPaths()

This method returns the paths to the associated CAD part and root file. These are only available if the part was imported from one of the supported CAD softwares using the Associative Import capability. The root file can be the assembly file or the part file, depending on what which one was imported.

Returns:

paths: python:tuple

A sequence containing the path to the associated CAD part and assembly file

getCADParameters()

This method returns the names and values of the CAD parameters associated with the part. These are only available if the part was imported from one of the supported CAD softwares using the Associative Import capability, and if the parameter names defined in that CAD software are prefixed with the string ABQ.

Returns:

paras: python:dict

A dictionary object representing a map of the name of the parameter and its associated value.

getCentroid(faces: tuple[Face], cells: tuple[Face], relativeAccuracy: float = 0)

Depending on the arguments provided, this method returns the following:

• The location of the centroid of a given face or group of faces.

• The location of the centroid of a given cell or group of cells.

faces

A sequence of Face objects whose centroid the method will calculate. The arguments faces and cells are mutually exclusive.

cells

A sequence of Face objects whose centroid the method will calculate. The arguments faces and cells are mutually exclusive.

relativeAccuracy

A Float specifying that the centroid computation should stop when the specified relative accuracy has been achieved. The default value is 0.000001 (0.0001%).

Returns:

centroid: python:tuple[python:float]

A sequence of Floats specifying the X-, Y-, and Z-coordinates of the centroid.

getCoordinates(entity: str, csys: DatumCsys)

This method returns the coordinates of specified point.

Parameters:

entity

A ConstrainedSketchVertex, Datum point, MeshNode, or ReferencePoint specifying the entity to query.

csys

A DatumCsys object specifying the desired coordinate system of the returned coordinates. By default, coordinates are given in the global coordinate system.

Returns:

A python:tuple of 3 Floats representing the coordinates of the specified point.

getCurvature(edges: tuple[Edge], samplePoints: int = 100)

This method returns the maximum curvature of a given edge or group of edges. For an arc, the curvature is constant over the entire edge, and equal to the inverse of the radius. For a straight line, the curvature is constant and equal to 0. For a spline edge, the curvature varies over a range, and this methods computes the maximum.

Parameters:

edges

A sequence of Edge objects whose curvature the method will calculate.

samplePoints

An Int specifying the number of points along each edge at which the curvature will be computed. The higher the number of sample points, the better the accuracy of the computation. The default value is 100.

Returns:

curvature: python:float

A Float specifying the maximum curvature.

getDistance(entity1: str, entity2: str)

Depending on the arguments provided, this method returns one of the following:

• The distance between two points.

• The minimum distance between a point and an edge.

• The minimum distance between two edges.

Parameters:

entity1

A ConstrainedSketchVertex, Datum point, MeshNode, or Edge specifying the first entity from which to measure.

entity2

A ConstrainedSketchVertex, Datum point, MeshNode, or Edge specifying the second entity to which to measure.

Returns:

distance: python:float

A Float specifying the distance between entity1 and entity2.

getFeatureCells(name: str)

This method returns a sequence of Cell objects that are created by the given feature.

Parameters:

name

A string specifying the feature name.

Returns:

cells: python:tuple[Cell]

Sequence of Cell objects.

Raises:

• An exception occurs if a feature with the given name does not exist.

  Error : Incorrect feature name.

getFeatureEdges(name: str)

This method returns a sequence of Edge objects that are created by the given feature.

Parameters:

name

A string specifying the feature name.

Returns:

edges: python:tuple[Edge]

Sequence of Edge objects.

Raises:

• An exception occurs if a feature with the given name does not exist.

  Error : Incorrect feature name.

getFeatureFaces(name: str)

This method returns a sequence of Face objects that are created by the given feature.

Parameters:

name

A string specifying the feature name.

Returns:

faces: python:tuple[Face]

Sequence of Face objects.

Raises:

• An exception occurs if a feature with the given name does not exist.

  Error : Incorrect feature name.

getFeatureVertices(name: str)

This method returns a sequence of ConstrainedSketchVertex objects that are created by the given feature.

Parameters:

name

A string specifying the feature name.

Returns:

vertices: python:tuple[ConstrainedSketchVertex]

Sequence of ConstrainedSketchVertex objects.

Raises:

• An exception occurs if a feature with the given name does not exist.

  Error : Incorrect feature name.

getLength(edges: tuple[Edge])

This method returns the length of a given edge or group of edges.

Parameters:

edges

A sequence of Edge objects whose total length the method will calculate.

Returns:

length: python:float

A Float specifying the total length

getMassProperties(regions: str = '', relativeAccuracy: SymbolicConstantType = 'LOW', useMesh: BooleanType = False, specifyDensity: BooleanType = False, density: str = '', specifyThickness: BooleanType = False, thickness: str = '', miAboutCenterOfMass: BooleanType = True, miAboutPoint: tuple = ())

This method returns the mass properties of a part or region. Only beams, trusses, shells, solids, point, nonstructural mass, and rotary inertia elements are supported.

Parameters:

regions

A MeshElementArray, CellArray, FaceArray, or EdgeArray specifying the regions whose mass properties are to be queried. The whole part is queried by default.

relativeAccuracy

A SymbolicConstant specifying the relative accuracy for geometry computation. Possible values are LOW, MEDIUM and HIGH. The default value is LOW.

useMesh

A Boolean specifying whether the mesh should be used in the computation if the geometry is meshed. The default value is False.

specifyDensity

A Boolean specifying whether a user-specified density should be used in regions with density errors such as undefined material density. The default value is False.

density

A double value specifying the user-specified density value to be used in regions with density errors. The user-specified density should be greater than 0.

specifyThickness

A Boolean specifying whether a user-specified thickness should be used in regions with thickness errors such as undefined thickness. The default value is False.

thickness

A double value specifying the user-specified thickness value to be used in regions with thickness errors. The user-specified thickness should be greater than 0.

miAboutCenterOfMass

A Boolean specifying if the moments of inertia should be evaluated about the center of mass. The default value is True.

miAboutPoint

A tuple of three floats specifying the coordinates of the point about which to evaluate the moment of inertia. By default if the moments of inertia are not being evaluated about the center of mass, they will be evaluated about the origin.

Returns:

properties: python:dict

A Dictionary object with the following items: area: None or a Float specifying the sum of the area of the specified faces. The area is computed only for one side for shells. areaCentroid: None or a tuple of three Floats representing the coordinates of the area centroid. volume: None or a Float specifying the volume of the specified regions. volumeCentroid: None or a tuple of three Floats representing the coordinates of the volume centroid. massFromMassPerUnitSurfaceArea: None or a Float specifying the mass due to mass per unit surface area. mass: None or a Float specifying the mass of the specified regions. It is the total mass and includes mass from quantities such as mass per unit surface area. centerOfMass: None or a tuple of three Floats representing the coordinates of the center of mass. momentOfInertia: None or a tuple of six Floats representing the moments of inertia about the center of mass or about the point specified. warnings: A tuple of SymbolicConstants representing the problems encountered while computing the mass properties. Possible SymbolicConstants are: UNSUPPORTED_ENTITIES: Some unsupported entities exist in the specified region. The mass properties are computed only for beams, trusses, shells, solids, point and non-structural mass elements and rotary inertia elements. The mass properties are not computed for axisymmetric elements, springs, connectors, gaskets or any other elements. MISSING_THICKNESS: For some regions, the section definitions are missing thickness values. ZERO_THICKNESS: For some regions, the section definitions have a zero thickness value. VARIABLE_THICKNESS: The nodal thickness or field thickness specified for some regions has been ignored. NON_APPLICABLE_THICKNESS: For some regions, the thickness value is not applicable to the corresponding sections specified on the regions. MISSING_DENSITY: For some regions, the section definitions are missing material density values. MISSING_MATERIAL_DEFINITION: For some regions, the material definition is missing. ZERO_DENSITY: For some regions, the section definitions have a zero material density value. UNSUPPORTED_DENSITY: For some regions, either a negative material density or a temperature dependent density has been specified, or the material value is missing for one or more plies in the composite section. SHELL_OFFSETS: For shells, this method does not account for any offsets specified. MISSING_SECTION_DEFINITION: For some regions, the section definition is missing. UNSUPPORTED_SECTION_DEFINITION: The section definition provided for some regions is not supported. REINFORCEMENTS: This method does not account for any reinforcements specified on the model. SMEARED_PROPERTIES: For regions with composite section assignments, the density is smeared across the thickness. The volume centroid and center of mass computations for a composite shell use a lumped mass approach where the volume and mass is assumed to be lumped in the plane of the shell. As a result of these approximations the volume centroid, center of mass and moments of inertia may be slightly inaccurate for regions with composite section assignments. UNSUPPORTED_NON_STRUCTURAL_MASS_ENTITIES: This method does not account for any non-structural mass on wires. INCORRECT_MOMENT_OF_INERTIA: For geometry regions with non-structural mass per volume, the non-structural mass is assumed to be a point mass at the centroid of the regions. Thus, the moments of inertia may be inaccurate as the distribution of the non-structural mass is not accounted for. Use the mesh for accurately computing the moments of inertia. MISSING_BEAM_ORIENTATIONS: For some regions with beam section assignments, the beam section orientations are missing. UNSUPPORTED_BEAM_PROFILES: This method supports the Box, Pipe, Circular, Rectangular, Hexagonal, Trapezoidal, I, L, T, Arbitrary, and Tapered beam profiles. Any other beam profile is not supported. TAPERED_BEAM_MI: Moment of inertia calculations for tapered beams are not accurate. SUBSTRUCTURE_INCORRECT_PROPERTIES: The user assigned density and thickness is not considered for substructures. UNSUPPORTED_NON_STRUCTURAL_MASS_PROPORTIONAL: Non-structural mass with Mass Proportional distribution is not supported. Results are computed using Volume Proportional distribution.

getPerimeter(faces: tuple[Face])

This method returns the total perimeter of a given face or group of faces. All faces need to be on the same part. If the specified faces have shared edges, these edges are excluded from the computation, thus providing the length of the outer perimeter of the specified faces.

Parameters:

faces

A sequence of Face objects whose perimeter the method will calculate.

Returns:

perimeter: python:float

A Float specifying the perimeter

getVolume(cells: tuple[Cell], relativeAccuracy: float = 0)

This method returns the volume area of a given cell or group of cells.

Parameters:

cells

A sequence of Cell objects whose volume the method will calculate.

relativeAccuracy

A Float specifying the relative accuracy of the computation. The default value is 0.000001 (0.0001%).

Returns:

volume: python:float

A Float specifying the sum of the areas of the given faces

isAlignedWithSketch()

This method checks if the normal of an analytical rigid surface part is aligned with that of its sketch.

Returns:

A Boolean value of python:True if the part is aligned with the sketch and python:False if it is not

aligned.

Raises:

• If the part is not an analytical rigid part:

  AbaqusException: Can only be used with analytical rigid parts.

printAssignedSections()

This method prints information on each section that has been assigned to a region of the part.

projectEdgesOntoSketch(sketch: str, edges: tuple, constrainToBackground: BooleanType = True)

This method projects the selected edges of a part onto the specified ConstrainedSketch object. The edges appear as sketch geometry after projection. If the plane of projection is not parallel to the specified edge, the resultant sketch geometry may be of a different type. For example, a circular edge can be projected as an ellipse or a line depending on the angle of the plane of projection. By default, the projected edge will be constrained to the background geometry. You can remove this constraint by setting constrainToBackground to False.

Parameters:

sketch

The ConstrainedSketch object on which the edges are projected.

edges

A sequence of candidate edges to be projected onto the sketch.

constrainToBackground

A Boolean that determines whether the projected edges need to constrained to the background geometry. The default is True.

projectReferencesOntoSketch(sketch: str, filter: ~abaqusConstants.SymbolicConstantType = 'ALL_EDGES', upToFeature: ~abaqus.Part.Feature.Feature = <abaqus.Part.Feature.Feature object>, edges: tuple = (), vertices: tuple = ())

This method projects the vertices of specified edges, and datum points from the part onto the specified ConstrainedSketch object. The vertices and datum points appear on the sketch as reference geometry.

Parameters:

sketch

The ConstrainedSketch object on which the edges, vertices, and datum points are projected.

filter

A SymbolicConstant specifying how to limit the amount of projection. Possible values are ALL_EDGES and COPLANAR_EDGES. If *filter*=COPLANAR_EDGES, edges that are coplanar to the sketching plane are the only candidates for projection. The default value is ALL_EDGES.

upToFeature

A Feature object specifying a marker in the feature-based history of the part. Abaqus/CAE projects onto the sketch only the part entities that were created before the feature specified by this marker. By default, part entities in features created before the sketch you are editing are candidates for projection.

edges

A sequence of candidate edges whose vertices need to be projected onto the sketch. By default, all edges specified by the filter argument are candidates for projection.

vertices

A sequence of candidate vertices to be projected onto the sketch. By default, all vertices are candidates for projection.

queryAttributes(printResults: BooleanType = 0)

This method prints the following information about a part:

• the name, modeling space, and analysis type; and

• whether twist is included (only available when the modeling space is axisymmetric and

the analysis type is deformable); and

• the number of vertices, edges, faces and cells if applicable.

Parameters:

printResults

A Boolean which specifies whether the above information is to be printed. The default value is True

Returns:

attributes: python:dict

A Dictionary object with string keys and integer values which returns the above information with the keys being numVertices, numEdges, numFaces, numCells, numWiredEdges, numShellFaces and numSolidFaces.

queryCachedStates()

This method displays the position of geometric states relative to the sequence of features in the part cache. The output is displayed in the message area.

queryDisjointPlyRegions()

This method provides a list of all composite plys in the current part which have disjoint regions.

queryGeometry(relativeAccuracy: float = 0, printResults: BooleanType = True)

This method prints the following information about a part:

• the name, modeling space, and analysis type;

• whether twist is included (only available when the modeling space is axisymmetric and

the analysis type is deformable);

• a 3D point representing the minimum of the part’s bounding box;

• a 3D point representing the maximum of the part’s bounding box;

• a 3D point representing the part’s centroid (only on 3D solid parts); and

• the volume (only on 3D solid parts).

Parameters:

relativeAccuracy

A Float specifying that the property computations should stop when the specified relative accuracy has been achieved. The default value is 0.000001 (0.0001%).

printResults

A Boolean which specifies whether the above information is to be printed. The default value is True.

Returns:

geometry: python:dict

A Dictionary object with string keys, which returns the above information with the keys being name, space, type, volume, centroid, category and boundingBox.

queryRegionsMissingSections()

This method returns all regions in the part that do not have a section assignment but require one for analysis.

Returns:

region: Region

A Region object, or None

regenerate()

This method regenerates a part. When you modify features, it may be convenient to postpone regeneration until you make all your changes, since regeneration can be time consuming.

regenerationWarnings()

This method prints any regeneration warnings associated with the features.

removeInvalidGeometry()

Removes all invalid entities from the part, leaving a valid part. This is not recorded as a feature in the feature list, therefore it should be used on parts that have a single feature (such as an imported part). Note:This may remove valid entities that are connected to invalid ones. You can identify invalid entities using the query toolset before using this command.

restore()

This method restores the parameters of all features in the assembly to the value they had before a failed regeneration. Use the restore method after a failed regeneration, followed by a regenerate command.

resumeAllFeatures()

This method resumes all the suppressed features in the part.

resumeFeatures(featureNames: tuple)

This method resumes the specified suppressed features in the part.

Parameters:

featureNames

A tuple of names of features which are to be resumed.

resumeLastSetFeatures()

This method resumes the last set of features to be suppressed in the part.

saveGeometryCache()

This method caches the current geometry. Caching the current geometry improves regeneration performance.

setAssociatedCADPaths(partFile: str = '', rootFile: str = '')

This method sets the paths to the associated CAD part and root file. This method is only available if the part was imported from one of the supported CAD softwares using the Associative Import capability. The root file can be the assembly file or the part file, depending on the one that was imported. This method can be used to specify the new paths when the CAD data is moved to a different directory.

Parameters:

partFile

A String specifying the name of the associated CAD part file.

rootFile

A String specifying the name of the root associated CAD file. This can be the same as the part file or can be the assembly file, depending on the one that was imported.

setValues(*args, **kwargs)

This method modifies the Part object.

Raises:

RangeError

smoothNodes(nodes: tuple[MeshNode])

This method smooths the given nodes of a native mesh, moving them locally to a more optimal location that improves the quality of the mesh

Parameters:

nodes

A sequence of MeshNode objects or a Set object containing nodes.

suppressFeatures(featureNames: tuple)

This method suppresses the given features.

Parameters:

featureNames

A tuple of names of features which are to be suppressed in the part.

writeAcisFile(fileName: str, version: float | None = None)

This method exports the geometry of the part to a named file in ACIS format.

Parameters:

fileName

A String specifying the name of the file to which to write.

version

A Float specifying the ACIS version. For example, the Float 12.0 corresponds to ACIS Version 12.0. The default value is the current version of ACIS.

Raises:

• If the part is an orphan mesh part:

  Cannot export orphan mesh parts to ACIS.

writeCADParameters(paramFile: str, modifiedParams: tuple = (), updatePaths: str = '')

This method writes the parameters that were imported from the CAD system to a parameter file.

Parameters:

paramFile

A String specifying the parameter file name.

modifiedParams

A tuple of tuples each containing the part name, the parameter name, and the modified parameter value. Default is an empty tuple.

updatePaths

A Bool specifying whether to update the path of the CAD model file specified in the parameterFile to the current directory, if the CAD model is present in the current directory.

writeIgesFile(fileName: str, flavor: SymbolicConstantType)

This method exports the geometry of the part to a named file in IGES format.

Parameters:

fileName

A String specifying the name of the file to which to write.

flavor

A SymbolicConstant specifying a particular flavor of IGES. Possible values are STANDARD, AUTOCAD, SOLIDWORKS, JAMA, and MSBO.

Raises:

• If the part is an orphan mesh part:

  Cannot export orphan mesh parts to IGES.

writeStepFile(fileName: str)

This method exports the geometry of the part to a named file in STEP format.

Parameters:

fileName

A String specifying the name of the file to which to write.

Raises:

• If the part contains no geometry:

  Parterror: Cannot export orphan mesh parts to STEP.

writeVdaFile(fileName: str)

This method exports the geometry of the part to a named file in VDA-FS format.

Parameters:

fileName

A String specifying the name of the file to which to write.

Raises:

• If the part is an orphan mesh part:

  Cannot export orphan mesh parts to VDA-FS.

Object features

Part

class Part(name: str, dimensionality: SymbolicConstantType, type: SymbolicConstantType, twist: BooleanType = OFF)

class Part(name: str, objectToCopy: str, scale: float = 1, mirrorPlane: SymbolicConstantType = NONE, compressFeatureList: BooleanType = OFF, separate: BooleanType = OFF)

The Part object defines the physical attributes of a structure. Parts are instanced into the assembly and positioned before an analysis.

Notes

This object can be accessed by:

import part
mdb.models[name].parts[name]

Attributes:

geometryValidity: Boolean

A Boolean specifying the validity of the geometry of the part. The value is computed, but it can be set to ON to perform feature and mesh operations on an invalid part. There is no guarantee that such operations will work if the part was originally invalid.

isOutOfDate: int

An Int specifying that feature parameters have been modified but that the part has not been regenerated. Possible values are 0 and 1.

timeStamp: float

A Float specifying when the part was last modified.

vertices: VertexArray

A VertexArray object specifying all the vertices in the part.

ignoredVertices: IgnoredVertexArray

An IgnoredVertexArray object specifying all the ignored vertices in the part.

edges: EdgeArray

An EdgeArray object specifying all the edges in the part.

ignoredEdges: IgnoredEdgeArray

An IgnoredEdgeArray object specifying all the ignored edges in the part.

faces: FaceArray

A FaceArray object specifying all the faces in the part.

cells: CellArray

A CellArray object specifying all the cells in the part.

features: dict[str, Feature]

A repository of Feature objects specifying all the features in the part.

featuresById: dict[str, Feature]

A repository of Feature.:py:class:~abaqus.Assembly.Feature.Feature`.:py:class:~abaqus.Assembly.:py:class:`~abaqus.Assembly.Feature.Feature.:py:class:~abaqus.Assembly.Feature.Feature`` objects specifying all Feature.:py:class:~abaqus.Assembly.Feature.Feature`.:py:class:~abaqus.Assembly.:py:class:`~abaqus.Assembly.Feature.Feature.:py:class:~abaqus.Assembly.Feature.Feature`` objects in the` part. The Feature.:py:class:~abaqus.Assembly.Feature.Feature`.:py:class:~abaqus.Assembly.:py:class:`~abaqus.Assembly.Feature.Feature.:py:class:~abaqus.Assembly.Feature.Feature`` objects in the` featuresById repository are the` same as the` Feature.:py:class:~abaqus.Assembly.Feature.Feature`.:py:class:~abaqus.Assembly.:py:class:`~abaqus.Assembly.Feature.Feature.:py:class:~abaqus.Assembly.Feature.Feature`` objects in the` features repository. However, the` key to the` objects in the` featuresById repository is an integer specifying the` ID, whereas the` key to the` objects in the` features repository is a string specifying the` name.

datums: list[Datum]

A repository of Datum objects specifying all the datums in the part.

elements: MeshElementArray

A MeshElementArray object specifying all the elements in the part.

faces: dict[str, MeshFace]

A repository of MeshFace objects specifying all the element faces in the part. For a given element and a given face index within that element, the corresponding MeshFace object can be retrieved from the repository by using the key calculated as (i*8 + j), where i and j are zero-based element and face indices, respectively.

elementFaces: MeshFaceArray

A MeshFaceArray object specifying all the unique element faces in the part.

nodes: MeshNodeArray

A MeshNodeArray object specifying all the nodes in the part.

retainedNodes: MeshNodeArray

A MeshNodeArray object specifying all the retained nodes in the substructure part.

sets: dict[str, Set]

A repository of Set objects specifying for more information, see Set.

allSets: dict[str, Set]

A repository of Set objects specifying the contents of the all:py:class:`~abaqus.Region.Set.Set`s repository is the same as the contents of the sets repository.

allInternalSets: dict[str, Set]

A repository of Set objects specifying picked regions.

surfaces: dict[str, Surface]

A repository of Surface objects specifying for more information, see Surface.

allSurfaces: dict[str, Surface]

A repository of Surface objects specifying the contents of the all:py:class:`~abaqus.Region.Surface.Surface`s repository is the same as the contents of the surfaces repository.

allInternalSurfaces: dict[str, Surface]

A repository of Surface objects specifying picked regions.

skins: dict[str, Skin]

A repository of Skin objects specifying the skins created on the part.

stringers: dict[str, Stringer]

A repository of Stringer objects specifying the stringers created on the part.

referencePoints: ReferencePoints

A repository of ReferencePoint objects.

engineeringFeatures: EngineeringFeature

An EngineeringFeature object.

sectionAssignments: SectionAssignmentArray

A SectionAssignmentArray object.

materialOrientations: MaterialOrientationArray

A MaterialOrientationArray object.

compositeLayups: dict[str, CompositeLayup]

A repository of CompositeLayup objects.

edges: dict[str, MeshEdge]

A repository of MeshEdge.:py:class:~abaqus.Mesh.MeshEdge.MeshEdge` objects specifying all the element edges in the part. For a given element and a given edge index on a given face within that element, the corresponding MeshEdge.:py:class:~abaqus.Mesh.MeshEdge.MeshEdge` object can be retrieved from the repository by using the key calculated as (i*32 + j*4 + k), where i, j, and k are zero-based element, face, and edge indices, respectively.

elementEdges: MeshEdgeArray

A MeshEdgeArray object specifying all the unique element edges in the part.

AddCells(faceList: tuple[Face], flipped: BooleanType = 0)

This method tries to convert a shell entity to a solid entity. The conversion is not always successful.

Parameters:

faceList

A sequence of Face objects specifying the faces bounding the cell to add.

flipped

A Boolean specifying the direction of feature creation. The possible values are True and False. The default is True indicating that the direction is opposite to the face normal. When multiple faces are selected, Abaqus attempts to create cells on both sides of the selected faces and ignores the flipped argument.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

AnalyticRigidSurf2DPlanar(sketch: ConstrainedSketch)

This method creates a first Feature object for an analytical rigid surface by creating a planar wire from the given ConstrainedSketch object.

Parameters:

sketch

A ConstrainedSketch object specifying the planar wire.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

AnalyticRigidSurfExtrude(sketch: ConstrainedSketch, depth: float = 1)

This method creates a first Feature object for an analytical rigid surface by extruding the given ConstrainedSketch object by the given depth, creating a surface.

Parameters:

sketch

A ConstrainedSketch object specifying the planar wire.

depth

A Float specifying the extrusion depth. The default value is 1.0.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

AnalyticRigidSurfRevolve(sketch: ConstrainedSketch)

This method creates a first Feature object for an analytical rigid surface by revolving the given ConstrainedSketch object by 360° about the Y-axis.

Parameters:

sketch

A ConstrainedSketch object specifying the surface to be revolved.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

AssignMidsurfaceRegion(cellList: tuple[Cell])

This method assign a mid-surface property to sequence of Cell objects. If a reference representation of the part does not exist, it creates one. It also copies the cells to the reference representation and deletes the cells from the active representation of the part.

Parameters:

cellList

A sequence of Cell objects specifying the regions that will be used for mid-surface construction. These regions will be copied to the reference representation of the part.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

AttachmentPoints(name: str, points: float, projectionMethod: SymbolicConstantType = 'PROJECT_BY_PROXIMITY', projectOnFaces: tuple[Face] = (), projectOnElementFaces: tuple[MeshFace] = (), projectionDirStartPt: float | None = None, projectionDirEndPt: float | None = None, setName: str = '')

This method creates an attachment points Feature. Attachment points may be created using datum points, vertices, reference points, attachment points, interesting points, orphan mesh nodes or coordinates. Optionally, the attachment points can be projected on geometric faces or element faces.

Parameters:

name

A String specifying a unique Feature name.

points

A tuple of points. Each point can be a ConstrainedSketchVertex, Datum point, Reference point, Attachment point, orphan mesh Node, Interesting point object, or a tuple of Floats representing the coordinates of a point.

projectionMethod

A SymbolicConstant specifying the projection method. Possible values are PROJECT_BY_PROXIMITY and PROJECT_BY_DIRECTION. The default value is PROJECT_BY_PROXIMITY.

projectOnFaces

A sequence of Face objects specifying the geometry faces onto which the points are to be projected.

projectOnElementFaces

A sequence of MeshFace objects specifying the orphan mesh element faces onto which the points are to be projected.

projectionDirStartPt

A point specifying the start point of the projection direction. The point can be a ConstrainedSketchVertex, Datum point, Reference point, Attachment point, orphan mesh Node, Interesting point object, or a tuple of Floats representing the coordinates of a point.

projectionDirEndPt

A point specifying the end point of the projection direction. The point can be a ConstrainedSketchVertex, Datum point, Reference point, Attachment point, orphan mesh Node, Interesting point object, or a tuple of Floats representing the coordinates of a point.

setName

A String specifying a unique set name.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

AttachmentPointsAlongDirection(name: str, startPoint: float, pointCreationMethod: SymbolicConstantType, endPoint: float | None = None, direction: str = '', spacing: str = '', numPtsAlongDir: str = '', numPtsBetweenPts: str = '', createPtAtStartPt: BooleanType = True, createPtAtEndPt: BooleanType = True, projectionMethod: SymbolicConstantType = 'PROJECT_BY_PROXIMITY', projectOnFaces: tuple[Face] = (), projectOnElementFaces: tuple[MeshFace] = (), projectionDirStartPt: float | None = None, projectionDirEndPt: float | None = None, flipDirection: BooleanType = 0, setName: str = '')

This method creates a Feature object by creating attachment points along a direction or between two points. A Datum point, a ConstrainedSketchVertex, a Reference point, an Attachment point, an Interesting point, or an orphan mesh Node can be specified as the start or end point. The direction can be specified using a straight edge or a datum axis.

Parameters:

name

A String specifying a unique Feature name.

startPoint

A point specifying the start point of the direction along which to create points. The point can be a ConstrainedSketchVertex, Datum point, Reference point, Attachment point, orphan mesh Node, Interesting point object, or a tuple of Floats representing the coordinates of a point.

pointCreationMethod

A SymbolicConstant specifying the point creation method. Possible values are AUTO_FIT, NUM_PTS_ALONG_DIR, and NUM_PTS_BETWEEN_PTS.

endPoint

A point specifying the end point if creating points between two points. The point can be a ConstrainedSketchVertex, Datum point, Reference point, Attachment point, orphan mesh Node, Interesting point object, or a tuple of Floats representing the coordinates of a point.

direction

The direction can be specified by a straight edge or a datum axis.

spacing

A float specifying the spacing to be used between two points.

numPtsAlongDir

An integer specifying the number of points to be created along the specified direction.

numPtsBetweenPts

An integer specifying the number of points to be created between the start and end points.

createPtAtStartPt

A Boolean specifying whether to create an attachment point at the start point. The default value is True.

createPtAtEndPt

A Boolean specifying whether to create an attachment point at the end point. The default value is True.

projectionMethod

A SymbolicConstant specifying the projection method. Possible values are PROJECT_BY_PROXIMITY and PROJECT_BY_DIRECTION. The default value is PROJECT_BY_PROXIMITY.

projectOnFaces

A sequence of Face objects specifying the geometry faces onto which the points are to be projected.

projectOnElementFaces

A sequence of MeshFace objects specifying the orphan mesh element faces onto which the points are to be projected.

projectionDirStartPt

A point specifying the start point of the projection direction. The point can be a ConstrainedSketchVertex, Datum point, Reference point, Attachment point, orphan mesh Node, Interesting point object, or a tuple of Floats representing the coordinates of a point.

projectionDirEndPt

A point specifying the end point of the projection direction. The point can be a ConstrainedSketchVertex, Datum point, Reference point, Attachment point, orphan mesh Node, Interesting point object, or a tuple of Floats representing the coordinates of a point.

flipDirection

A Boolean specifying if the direction along which the attachment points are created should be reversed. This argument is valid only when *pointCreationMethod*=NUM_PTS_ALONG_DIR.

setName

A String specifying a unique set name.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

AttachmentPointsOffsetFromEdges(name: str, edges: tuple, startPoint: str = '', flipDirection: str = '', pointCreationMethod: SymbolicConstantType | None = None, numberOfPoints: str = '', spacingBetweenPoints: str = '', offsetFromStartPoint: str = 0, offsetFromEndPoint: str = 0, spacingMethod: SymbolicConstantType = 'AUTO_FIT_PTS', patterningMethod: SymbolicConstantType | None = None, referenceFace: str = '', startPointForPatternDirection: float | None = None, endPointForPatternDirection: float | None = None, offsetFromEdges: str = '', numberOfRows: str = 1, spacingBetweenRows: str = '', projectionMethod: SymbolicConstantType = 'PROJECT_BY_PROXIMITY', projectOnFaces: tuple[Face] = (), projectOnElementFaces: tuple[MeshFace] = (), projectionDirStartPt: float | None = None, projectionDirEndPt: float | None = None, setName: str = '')

This method creates a Feature object by creating attachment points along or offset from one or more connected edges.

Parameters:

name

A String specifying a unique Feature name.

edges

A sequence of connected Edge objects specifying the geometry edges from which to offset the points.

startPoint

A ConstrainedSketchVertex of the selected edges that specifies the point from which to create points. This point can be one of the two end vertices of the connected edges. In case of edges forming a closed loop and having multiple vertices, this point can be any one of the vertices on the edges.

flipDirection

This parameter is required to indicate the direction in which to create the points. This parameter is required only in case of edges forming a closed loop.

pointCreationMethod

A SymbolicConstant specifying the point creation method. Possible values are BY_NUMBER or BY_SPACING.

numberOfPoints

An integer specifying the number of points to be created along the selected edges.

spacingBetweenPoints

A float specifying the spacing to be used between two points while creating the points between the start and end points of the edges.

offsetFromStartPoint

A float specifying the distance by which to offset the first point from the start vertex of the edge chain. The default value is 0.0.

offsetFromEndPoint

A float specifying the distance by which to offset the last point from the end vertex of the edge chain. This parameter should be specified only if the point creation method is BY_NUMBER. The default value is 0.0.

spacingMethod

A SymbolicConstant specifying the spacing method. Possible values are AUTO_FIT_PTS or SPECIFY_NUM_PTS. The default value is AUTO_FIT_PTS.

patterningMethod

A SymbolicConstant specifying the method to pattern of points. Possible values are PATTERN_ORTHOGONALLY or PATTERN_ALONG_DIRECTION.

referenceFace

A geometry Face object adjacent to one of the edges from which to offset the points to create a pattern of points when the PATTERN_ORTHOGONALLY method is chosen for patterning. The face is used to identify the patterning direction. If the number of rows is one and the initial offset is zero, the reference face may not be specified.

startPointForPatternDirection

A point specifying the start point of the direction along which to create a pattern of points when the PATTERN_ALONG_DIRECTION method is chosen for patterning. The point can be a ConstrainedSketchVertex, Datum point, Reference point, Attachment point, orphan mesh Node, Interesting point object, or a tuple of Floats representing the coordinates of a point.

endPointForPatternDirection

A point specifying the end point of the direction along which to create a pattern of points when the PATTERN_ALONG_DIRECTION method is chosen for patterning. The point can be a ConstrainedSketchVertex, Datum point, Reference point, Attachment point, orphan mesh Node, Interesting point object, or a tuple of Floats representing the coordinates of a point.

offsetFromEdges

A float specifying the distance by which to offset the first row of points from the edges.

numberOfRows

An integer specifying the number of rows of points to be created for the pattern. The default value is 1.

spacingBetweenRows

A float specifying the spacing to be used between two rows while creating a pattern of points.

projectionMethod

A SymbolicConstant specifying the projection method. Possible values are PROJECT_BY_PROXIMITY and PROJECT_BY_DIRECTION. The default value is PROJECT_BY_PROXIMITY.

projectOnFaces

A sequence of Face objects specifying the geometry faces onto which the points are to be projected.

projectOnElementFaces

A sequence of MeshFace objects specifying the orphan mesh element faces onto which the points are to be projected.

projectionDirStartPt

A point specifying the start point of the projection direction. The point can be a ConstrainedSketchVertex, Datum point, Reference point, Attachment point, orphan mesh Node, Interesting point object, or a tuple of Floats representing the coordinates of a point.

projectionDirEndPt

A point specifying the end point of the projection direction. The point can be a ConstrainedSketchVertex, Datum point, Reference point, Attachment point, orphan mesh Node, Interesting point object, or a tuple of Floats representing the coordinates of a point.

setName

A String specifying a unique set name.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

AutoRepair()

This method carries out a sequence of geometry repair operations if it contains invalid entities. It is expected to improve the geometry, but it does not guarantee that the number of invalid entities will decrease. In some cases, it can also increase the number of invalid entities. Since a number of geometry repair operations and validity checks are performed, it could be a slow operation depending on the complexity of the geometry.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseShell(sketch: ConstrainedSketch)

This method creates a first Feature object by creating a planar shell from the given ConstrainedSketch object. The ConstrainedSketch object must define a closed profile.

Parameters:

sketch

A ConstrainedSketch object specifying the planar shell.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseShellExtrude(sketch: ConstrainedSketch, depth: float, draftAngle: float | None = None, pitch: float | None = None)

This method creates a first Feature object by extruding the given ConstrainedSketch object by the given depth, creating a shell. The ConstrainedSketch object can define either an open or closed profile.

Parameters:

sketch

A ConstrainedSketch object specifying the shape to be extruded.

depth

A Float specifying the extrusion depth. Possible values are Floats > 0.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

Returns:

A Feature object.

Raises:

RangeError

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseShellRevolve(sketch: ConstrainedSketch, angle: float, pitch: float | None = None, flipRevolveDirection: BooleanType = 0, flipPitchDirection: BooleanType = 0, moveSketchNormalToPath: BooleanType = 0)

This method creates a first Feature object by revolving the given ConstrainedSketch object by the given angle, creating a shell. The ConstrainedSketch object can define either an open or closed profile and an axis of revolution. The axis is defined by a single construction line.

Parameters:

sketch

A ConstrainedSketch object specifying the shape to be revolved.

angle

A Float specifying the revolve angle in degrees. Possible values are 0 ≤≤ angle ≤≤ 360.Note:If pitch >> 0, there is no upper limit for angle.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤≤ pitch ≤≤ 105. The default value, 0, implies a normal revolve.

flipRevolveDirection

A Boolean specifying whether to override the direction of feature creation. If *flipRevolveDirection*=OFF, the default direction of revolution is used. If *flipRevolveDirection*=ON, the revolve direction is reversed. The default value is OFF.

flipPitchDirection

A Boolean specifying whether to override the direction of translation. If *flipPitchDirection*=OFF, the direction of translation is given by the direction of the revolve axis. If *flipPitchDirection*=ON, the translation direction is reversed. The default value is OFF.

moveSketchNormalToPath

A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath*=OFF, the sketch plane remains parallel to the revolve axis. If *moveSketchNormalToPath*=ON, the sketch is moved to match the angle created by the *pitch before being revolved. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseShellSweep(sketch: ConstrainedSketch, path: ConstrainedSketch)

This method creates a first Feature object by sweeping the given section ConstrainedSketch object along the path defined by the path ConstrainedSketch object, creating a shell. The ConstrainedSketch object can define either an open or closed profile. The origin of the profile sketch is positioned at the start of the sweep path and swept perpendicular to the path. No checks are made for self-intersection.

Parameters:

sketch

A ConstrainedSketch object specifying the section to be swept.

path

A ConstrainedSketch object specifying the path of the sweep.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseSolidExtrude(sketch: ConstrainedSketch, depth: float, draftAngle: float | None = None, pitch: float | None = None)

This method creates a first Feature object by extruding the given ConstrainedSketch object by the given depth, creating a solid. The ConstrainedSketch object must define a closed profile.

Parameters:

sketch

A ConstrainedSketch object specifying the plane shape to be extruded.

depth

A Float specifying the extrusion depth. Possible values are 10–5 ≤≤ depth ≤≤ 105.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

Returns:

A Feature object.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseSolidRevolve(sketch: ConstrainedSketch, angle: float, pitch: float | None = None, flipRevolveDirection: BooleanType = 0, flipPitchDirection: BooleanType = 0, moveSketchNormalToPath: BooleanType = 0)

This method creates a first Feature object by revolving the given ConstrainedSketch object by the given angle, creating a solid. The ConstrainedSketch object must define a closed profile and an axis of revolution. The axis is defined by a single construction line.

Parameters:

sketch

A ConstrainedSketch object specifying the shape to be revolved.

angle

A Float specifying the revolve angle in degrees. Possible values are 10–4 ≤≤ angle ≤≤ 360.Note:If pitch >>0, there is no upper limit for angle.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤≤ pitch ≤≤ 105. The default value, 0, implies a normal revolve.

flipRevolveDirection

A Boolean specifying whether to override the direction of feature creation. If *flipRevolveDirection*=OFF, the default direction of revolution is used. If *flipRevolveDirection*=ON, the revolve direction is reversed. The default value is OFF.

flipPitchDirection

A Boolean specifying whether to override the direction of translation. If *flipPitchDirection*=OFF, the direction of translation is given by the direction of the revolve axis. If *flipPitchDirection*=ON, the translation direction is reversed. The default value is OFF.

moveSketchNormalToPath

A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath*=OFF, the sketch plane remains parallel to the revolve axis. If *moveSketchNormalToPath*=ON, the sketch is moved to match the angle created by the *pitch before being revolved. The default value is OFF.

Returns:

A Feature object.

Raises:

RangeError

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseSolidSweep(sketch: ConstrainedSketch, path: ConstrainedSketch)

This method creates a first Feature object by sweeping the given profile ConstrainedSketch object along the path defined by the path ConstrainedSketch object, creating a solid. The profile ConstrainedSketch object must define a closed profile. The origin of the profile sketch is positioned at the start of the sweep path and swept perpendicular to the path. No checks are made for self-intersection.

Parameters:

sketch

A ConstrainedSketch object specifying the profile to be swept.

path

A ConstrainedSketch object specifying the path of the sweep.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseWire(sketch: ConstrainedSketch)

This method creates a first Feature object by creating a planar wire from the given ConstrainedSketch object.

Parameters:

sketch

A ConstrainedSketch object specifying the planar wire.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BlendFaces(side1: tuple[abaqus.BasicGeometry.Edge.Edge], side2: tuple, method: ~abaqusConstants.SymbolicConstantType | None = None, path: ~abaqus.BasicGeometry.Edge.Edge = <abaqus.BasicGeometry.Edge.Edge object>)

This method creates a Feature object by creating new faces that blends two sets of faces.

Parameters:

side1

A sequence of Edge objects specifying one side of the blend. The edges must form a continuous chain without branches.

side2

A sequence of Edge or Face objects specifying the second side of the blend. If side2 contains Edge objects then they must form a continuous chain without branches.

method

A SymbolicConstant indicating a method for creating blends. This argument is a required argument if side2 contains Edge object and it is ignored if side2 contains Faceobjects. It can have one of the following values:TANGENT: The blend is tangent to the sides.SHORTEST_PATH: The blend connects the two sides based on linear interpolation between the two sides.SPECIFY_PATH: The blend connects the two sides along a specified path.

path

An Edge object that connects side1 to side2 and specifies the path for creating the blend. This argument is required if *method*=SPECIFY_PATH; otherwise, it is ignored.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Chamfer(length: float, edgeList: tuple[Edge])

This method creates an additional Feature object by chamfering the given list of edges with a given length.

Parameters:

length

A Float specifying the length of the chamfer.

edgeList

A sequence of Edge objects specifying the edges to chamfer.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

CompositeLayup(name: str, description: str = '', offsetType: SymbolicConstantType = 'GLOBAL', offsetField: str = '', offsetValues: float = 0, elementType: SymbolicConstantType = 'SHELL', symmetric: BooleanType = 0) → CompositeLayup

This method creates a CompositeLayup object.

Parameters:

name

A String specifying the repository key.

description

A String specifying a description of the composite layup.

offsetType

A SymbolicConstant specifying the method used to define the shell offset. If offsetType*=OFFSET_FIELD the *offsetField argument is required. This member is valid only if *elementType*=SHELL. Possible values are SINGLE_VALUE, MIDDLE_SURFACE, TOP_SURFACE, BOTTOM_SURFACE, OFFSET_FIELD, and GLOBAL. The default value is GLOBAL.

offsetField

A String specifying The name of the field specifying the offset. This member is valid only if *elementType*=SHELL. The default value is an empty string.

offsetValues

A Float specifying The offset of the shell section. This member is valid only if *elementType*=SHELL. The default value is 0.0.

elementType

A SymbolicConstant specifying the type of element in the composite layup. Possible values are SHELL, CONTINUUM_SHELL, and SOLID. The default value is SHELL.

symmetric

A Boolean specifying whether or not the layup should be made symmetric by the analysis. The default value is OFF.

Returns:

layup: CompositeLayup

A CompositeLayup object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].CompositeLayup

ConvertToAnalytical()

This method attempts to change entities into a simpler form that will speed up processing and make entities available during feature operations.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

ConvertToPrecise(method: SymbolicConstantType = 'RECOMPUTE_GEOMETRY')

This method attempts to change imprecise entities so that the geometry becomes precise.

Parameters:

method

A SymbolicConstant specifying the method to be used to convert the part to precise. Possible values are RECOMPUTE_GEOMETRY and TIGHTEN_GAPS. The default value is RECOMPUTE_GEOMETRY.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

CoverEdges(edgeList: tuple[Edge], tryAnalytical: BooleanType = False)

This method generates a face using the given edges as the face’s boundaries. The CoverEdges method generates a face by creating the geometry consisting of the underlying surface, associated edges, and vertices.

Parameters:

edgeList

A sequence of Edge objects specifying the edges that bound the new face.

tryAnalytical

A Boolean specifying whether the newly created face should be analytical or not. The default is False.

Returns:

A Feature object.

Raises:

• If the given boundary is not a closed loop:

  Parterror: Cannot find a closed loop

• If the given boundary contains a zero length component:

  Parterror: Cannot find a closed loop

• If the underlying surface is too difficult to fit:

  Parterror: Cannot construct face geometry

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Cut(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, sketchOrientation: SymbolicConstantType | None = None)

This method creates an additional Feature object by cutting a hole using the given ConstrainedSketch object.

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketch

A ConstrainedSketch object specifying the planar cut.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

CutExtrude(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketchOrientation: SymbolicConstantType, sketch: ConstrainedSketch, depth: float | None = None, upToFace: str = '', draftAngle: float | None = None, pitch: float | None = None, flipExtrudeDirection: BooleanType = 0)

This method creates an additional Feature object by extruding the given ConstrainedSketch object by the given depth and cutting away material in the solid and shell regions of the part. The ConstrainedSketch object must define a closed profile. The CutExtrude method creates a blind cut (using depth), an up-to-face cut (using upToFace), or a through-all cut (if depth and upToFace are not specified).

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM.

sketch

A ConstrainedSketch object specifying the planar sketch to be extruded.

depth

A Float specifying the extrusion depth. If depth is specified, the cut will be a blind cut. The default is to not specify a depth.

upToFace

A Face specifying the face up to which to cut. If upToFace is specified, the cut will be an up-to-face cut. The default is to not specify a face.Note:If neither depth nor upToFace is specified, the cut will be a through-all cut.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

flipExtrudeDirection

A Boolean specifying whether to override the direction of feature creation. If the value is OFF, it means use the direction defined by the sketchPlaneSide; if the value is ON, it means use the opposite direction to the one defined by sketchPlaneSide. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

CutLoft(loftsections: tuple, startCondition: SymbolicConstantType | None = None, endCondition: SymbolicConstantType | None = None, startTangent: float | None = None, startMagnitude: float | None = None, endTangent: float | None = None, endMagnitude: float | None = None, globalSmoothing: BooleanType = 0)

This method creates an additional Feature object by lofting between the given sections and cutting away material from the part. You define the sections using a sequence of edges from the part or an EdgeArray.

Parameters:

loftsections

A sequence of sequences of edges specifying the cross-sections to be lofted. Each outer sequence specifies a section through which the method will pass the loft feature. Each outer sequence can be defined as a sequence of edges or as an EdgeArray. The edges specifying a section must form a simple closed profile and must not contain multiple loops.

startCondition

A SymbolicConstant specifying the tangent direction at the start section of the loft feature. Possible values are NONE, NORMAL, RADIAL, and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the startCondition argument in conjunction with the endCondition argument.

endCondition

A SymbolicConstant specifying the tangent direction at the end section of the loft feature. Possible values are NONE, NORMAL, RADIAL, and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the endCondition argument in conjunction with the startCondition argument.

startTangent

A Float specifying the angle in degrees of the tangent with respect to the plane in which the start section lies. You must specify the startTangent argument if startCondition*=SPECIFIED. Possible values are 0.0 ≤≤ *startTangent ≤≤ 180.0.

startMagnitude

A Float specifying the magnitude of the startTangent. You must specify the startMagnitude argument if startCondition*=SPECIFIED. Possible values are 0.0 << *startMagnitude << 100.0.

endTangent

A Float specifying the angle in degrees of the tangent with respect to the plane in which the end section lies. You must specify the endTangent argument if startCondition*=SPECIFIED. Possible values are 0.0 ≤≤ *endTangent ≤≤ 180.0.

endMagnitude

A Float specifying the magnitude of the endTangent. This argument is to be used when the endCondition argument has the value SPECIFIED. Possible values are 0.0 << endMagnitude << 100.0.

globalSmoothing

A Boolean specifying whether each path defined in the paths argument is applied locally or globally.If the path is applied locally, its effect is felt only on faces created from the edges on the loftSections through which the paths pass through.If the path is applied globally, an averaging algorithm is applied over all the paths defined and is distributed over all the faces created.The default value is ON (globally).

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

CutRevolve(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketchOrientation: SymbolicConstantType, sketch: ConstrainedSketch, angle: float, pitch: float | None = None, flipRevolveDirection: BooleanType = 0, flipPitchDirection: BooleanType = 0, moveSketchNormalToPath: BooleanType = 0)

This method creates an additional Feature object by revolving the given ConstrainedSketch object by the given angle and cutting away material from the part. The ConstrainedSketch object must define a closed profile and an axis of revolution.

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM.

sketch

A ConstrainedSketch object specifying the planar sketch to be revolved.

angle

A Float specifying the angle in degrees to be revolved.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤≤ pitch ≤≤ 105. The default value, 0, implies a normal revolve.

flipRevolveDirection

A Boolean specifying whether to override the direction of feature creation. If *flipRevolveDirection*=OFF, the default direction of revolution is used. If *flipRevolveDirection*=ON, the revolve direction is reversed. The default value is OFF.

flipPitchDirection

A Boolean specifying whether to override the direction of translation. If *flipPitchDirection*=OFF, the direction of translation is given by the direction of the revolve axis. If *flipPitchDirection*=ON, the translation direction is reversed. The default value is OFF.

moveSketchNormalToPath

A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath*=OFF, the sketch plane remains parallel to the revolve axis. If *moveSketchNormalToPath*=ON, the sketch is moved to match the angle created by the *pitch before being revolved. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

CutSweep(path: str, profile: str, pathPlane: str = '', pathUpEdge: ~abaqus.BasicGeometry.Edge.Edge = <abaqus.BasicGeometry.Edge.Edge object>, pathOrientation: ~abaqusConstants.SymbolicConstantType | None = None, sketchPlane: str = '', sketchUpEdge: ~abaqus.BasicGeometry.Edge.Edge = <abaqus.BasicGeometry.Edge.Edge object>, sketchOrientation: ~abaqusConstants.SymbolicConstantType | None = None, draftAngle: float | None = None, pitch: float | None = None, profileNormal: ~abaqusConstants.BooleanType = 0, flipSweepDirection: ~abaqusConstants.BooleanType = 0)

This method creates an additional Feature object by sweeping the given ConstrainedSketch object along a path which may be a ConstrainedSketch or a sequence of Edge objects and cutting away material from the part. If the profile section is a ConstrainedSketch object, it must define a closed profile. The section sketch can be created at the normal plane at the start of the sweep path or it may be created on a Datum plane or a planar Face. No checks are made for self-intersection.

Parameters:

path

Path may either be a ConstrainedSketch object or a sequence of Edge objects specifying the path of the sweep.

profile

Profile may either be a ConstrainedSketch object or a Face object specifying the section to be swept.

pathPlane

A Datum plane object or a planar Face object. Only required when path is a ConstrainedSketch object.

pathUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the path sketch. Only required when path is a ConstrainedSketch object.

pathOrientation

A SymbolicConstant specifying the orientation of pathUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when path is a ConstrainedSketch object.

sketchPlane

A Datum plane object or a planar Face object specifying the plane on which to sketch the profile. Not required when profile is a Face object. When profile is chosen as a ConstrainedSketch object, user may or may not give this as input. If user does not give this as input, the normal plane at the start of the path will be the sketchPlane.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the profile sketch. Only required when profile is a ConstrainedSketch object.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when profile is a ConstrainedSketch object.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

profileNormal

A Boolean specifying whether to keep the profile normal same as original or varying through out the sweep path. When *profileNormal*=OFF, the profile normal will vary through out the sweep path. When *profileNormal*=ON, the profile normal will be same as original through out the sweep path. The default value is OFF.

flipSweepDirection

A Boolean specifying whether to flip the direction in which sweep operation will be performed. When *flipSweepDirection*=OFF, sweep operation will be performed in the direction of path direction. When *flipSweepDirection*=ON, sweep operation will be performed in the direction opposite to the path direction. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

DatumAxisByCylFace(face: str)

This method creates a Feature object and a DatumAxis object along the axis of a cylinder or cone.

Parameters:

face

A cylindrical or conical Face object.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumAxisByNormalToPlane(plane: str, point: int)

This method creates a Feature object and a DatumAxis object normal to the specified plane and passing through the specified point.

Parameters:

plane

A planar Face, an ElementFace, or a Datum object representing a datum plane.

point

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumAxisByParToEdge(edge: str, point: int)

This method creates a Feature object and a DatumAxis object parallel to the specified edge and passing through the specified point.

Parameters:

edge

A straight Edge, an ElementEdge, or a Datum object representing a datum axis.

point

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumAxisByPrincipalAxis(principalAxis: SymbolicConstantType)

This method creates a Feature object and a DatumAxis object along one of the three principal axes.

Parameters:

principalAxis

A SymbolicConstant specifying the principal axis. Possible values are XAXIS, YAXIS, and ZAXIS.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumAxisByThreePoint(point1: int, point2: int, point3: int)

This method creates a Feature object and a DatumAxis object normal to the circle described by three points and through its center.

Parameters:

point1

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point specifying the first point on the circle.

point2

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point specifying the second point on the circle.

point3

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point specifying the third point on the circle.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumAxisByThruEdge(edge: str)

This method creates a Feature object and a DatumAxis object along the specified edge.

Parameters:

edge

A straight Edge or an ElementEdge object.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumAxisByTwoPlane(plane1: str, plane2: str)

This method creates a Feature object and a DatumAxis object at the intersection of two planes.

Parameters:

plane1

A planar Face, an ElementFace, or a Datum object representing a datum plane.

plane2

A planar Face, an ElementFace, or a Datum object representing a datum plane.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumAxisByTwoPoint(point1: int, point2: int)

This method creates a Feature object and a DatumAxis object along the line joining two points.

Parameters:

point1

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

point2

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumCsysByDefault(coordSysType: SymbolicConstantType, name: str = '')

This method creates a Feature object and a DatumCsys object from the specified default coordinate system at the origin.

Parameters:

coordSysType

A SymbolicConstant specifying the default coordinate system to be used. Possible values are CARTESIAN, CYLINDRICAL, and SPHERICAL.

name

A String specifying the name of the DatumCsys.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumCsysByOffset(coordSysType: SymbolicConstantType, datumCoordSys: Datum, vector: tuple, point: str, name: str = '')

This method creates a Feature object and a DatumCsys object by offsetting the origin of an existing datum coordinate system to a specified point.

Parameters:

coordSysType

A SymbolicConstant specifying the type of coordinate system. Possible values are CARTESIAN, CYLINDRICAL, and SPHERICAL.

datumCoordSys

A Datum object representing a datum coordinate system from which to offset.

vector

A sequence of three Floats specifying the X-, Y-, and Z-offsets from datumCoordSys. The arguments vector and point are mutually exclusive, and one of them must be specified.

point

A ConstrainedSketchVertex, InterestingPoint, DatumPoint object or a sequence of three Floats specifying the X-, Y-, and Z-coordinates of a point in space. The point represents the origin of the new datum coordinate system. The arguments vector and point are mutually exclusive, and one of them must be specified.

name

A String specifying the name of the DatumCsys.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumCsysByThreePoints(coordSysType: SymbolicConstantType, origin: int, point1: int, point2: int, line1: str, line2: str, name: str = '')

This method creates a Feature object and a DatumCsys object from three points.

Parameters:

coordSysType

A SymbolicConstant specifying the type of coordinate system. Possible values are CARTESIAN, CYLINDRICAL, and SPHERICAL.

origin

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point specifying the origin of the coordinate system.

point1

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point specifying a point on the X-axis or the rr-axis. The point1 and line1 arguments are mutually exclusive. One of them must be specified.

point2

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point specifying a point in the X–Y plane or the rr–θθ plane. The point2 and line2 arguments are mutually exclusive. One of them must be specified.

line1

An Edge, an Element Edge, or a Datum object representing a datum axis specifying the X-axis or the rr-axis. The point1 and line1 arguments are mutually exclusive. One of them must be specified.

line2

An Edge, an Element Edge, or a Datum object representing a datum axis specifying a vector in the X–Y plane or the rr–θθ plane. The point2 and line2 arguments are mutually exclusive. One of them must be specified.

name

A String specifying the name of the DatumCsys.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumCsysByTwoLines(coordSysType: SymbolicConstantType, line1: str, line2: str, name: str = '')

This method creates a Feature object and a DatumCsys object from two orthogonal lines. The origin of the new datum coordinate system is placed at the intersection of the two lines.

Parameters:

coordSysType

A SymbolicConstant specifying the type of coordinate system. Possible values are CARTESIAN, CYLINDRICAL, and SPHERICAL.

line1

A straight Edge, an ElementEdge, or a Datum object representing a datum axis specifying the X-axis or the rr-axis.

line2

A straight Edge, an ElementEdge, or a Datum object representing a datum axis specifying a line in the X–Y plane or in the rr–θθ plane.

name

A String specifying the name of the DatumCsys.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumPlaneByLinePoint(line: str, point: int)

This method creates a Feature object and a DatumPlane object that pass through the specified line and through the specified point that does not lie on the line.

Parameters:

line

A straight Edge, an ElementEdge, or a Datum object representing a datum axis.

point

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumPlaneByPointNormal(point: int, normal: str)

This method creates a Feature object and a DatumPlane object normal to the specified line and running through the specified point.

Parameters:

point

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

normal

A straight Edge, an ElementEdge, or a Datum object representing a datum axis.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumPlaneByPrincipalPlane(principalPlane: SymbolicConstantType, offset: float)

This method creates a Feature object and a DatumPlane object through the origin along one of the three principal planes.

Parameters:

principalPlane

A SymbolicConstant specifying the principal plane. Possible values are XYPLANE, YZPLANE, and XZPLANE.

offset

A Float specifying the offset from the plane.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumPlaneByRotation(plane: str, axis: str, angle: float)

This method creates a Feature object and a DatumPlane object by rotating a plane about the specified axis through the specified angle.

Parameters:

plane

A planar Face, an ElementFace, or a Datum object representing a datum plane.

axis

A straight Edge, an ElementEdge, or a Datum object representing a datum axis.

angle

A Float specifying the angle in degrees to rotate the plane.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumPlaneByThreePoints(point1: int, point2: int, point3: int)

This method creates a Feature object and a DatumPlane object defined by passing through three points.

Parameters:

point1

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

point2

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

point3

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumPlaneByTwoPoint(point1: int, point2: int)

This method creates a Feature object and a DatumPlane object midway between two points and normal to the line connecting the points.

Parameters:

point1

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

point2

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumPointByCoordinate(coords: tuple)

This method creates a Feature object and a DatumPoint object at the point defined by the specified coordinates.

Parameters:

coords

A sequence of three Floats specifying the X-, Y-, and Z-coordinates of the datum point.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumPointByEdgeParam(edge: Edge, parameter: float)

This method creates a Feature object and a DatumPoint object along an edge at a selected distance from one end of the edge.

Parameters:

edge

An Edge object.

parameter

A Float specifying the distance along edge to the DatumPoint object. Possible values are 0 << parameter << 1.

Returns:

A Feature object.

Raises:

AbaqusException

RangeError

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumPointByMidPoint(point1: int, point2: int)

This method creates a Feature object and a DatumPoint object midway between two points.

Parameters:

point1

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

point2

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumPointByOffset(point: int, vector: tuple)

This method creates a Feature object and a DatumPoint object offset from an existing point by a vector.

Parameters:

point

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

vector

A sequence of three Floats specifying the X-, Y-, and Z-offsets from point.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumPointByOnFace(face: str, edge1: str, offset1: float, edge2: str, offset2: float)

This method creates a Feature object and a DatumPoint object on the specified face, offset from two edges.

Parameters:

face

A planar Face or a Datum object representing a datum plane.

edge1

A straight Edge or a Datum object representing a datum axis.

offset1

A Float specifying the offset from edge1.

edge2

A straight Edge or a Datum object representing a datum axis.

offset2

A Float specifying the offset from edge2.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumPointByProjOnEdge(point: int, edge: str)

This method creates a Feature object and a DatumPoint object along an edge by projecting an existing point along the normal to the edge.

Parameters:

point

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

edge

An Edge, an ElementEdge or a Datum object representing a datum axis.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

DatumPointByProjOnFace(point: int, face: Face)

This method creates a Feature object and a DatumPoint object on a specified face by projecting an existing point onto the face.

Parameters:

point

A ConstrainedSketchVertex, an InterestingPoint, a MeshNode, or a Datum object representing a datum point.

face

A Face object or a Datum object representing a datum plane.Note:Any other types of planes are not supported.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

EditSkin(name: str = '', faces: tuple[Face] = (), edges: tuple[Edge] = (), elementFaces: tuple[MeshFace] = (), elementEdges: tuple[MeshEdge] = ()) → Skin

This method modifies underlying entities of the selected skin. At least one of the optional arguments needs to be specified.

Parameters:

name

A String specifying the repository key. The default value is an empty string.

faces

A sequence of Face objects specifying the faces on which skins should be created. Applicable to three and two-dimensional parts.

edges

A sequence of Edge objects specifying the edges on which skins should be created. Applicable to axisymmetric parts.

elementFaces

A sequence of MeshFace objects specifying the mesh faces on which skins should be created. Applicable to three and two-dimensional parts.

elementEdges

A sequence of MeshEdge objects specifying the mesh edges on which skins should be created. Applicable to axisymmetric parts.

Returns:

skin: Skin

A Skin object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].EditSkin

ExtendFaces(faces: tuple[Face] = (), extendAlong: tuple[Edge] = (), distance: float | None = None, upToFaces: tuple[Face] = (), trimToExtendedTargetSurfaces: BooleanType = True, upToReferenceRep: BooleanType = 0)

This method extends faces along its free edges by offsetting the external edges along the surfaces. One of distance, upToReferenceRep, or upToFaces must be used to specify how far the faces need to be extended.

Parameters:

faces

A sequence of Face objects specifying the faces to be extended. The faces cannot belong to the reference representation. The faces and extendAlong arguments are mutually exclusive. One of them must be specified.

extendAlong

A sequence of Edge objects specifying the edges where to extend the faces. Only free edges are considered. The interior edges will be ignored. The faces and extendAlong arguments are mutually exclusive. One of them must be specified.

distance

A Float indicating the distance to extend the faces along the edges. Either distance, upToReferenceRep, or upToFaces must be specified.

upToFaces

A sequence of Face objects specifying the faces that the selected faces should be extended up to.

trimToExtendedTargetSurfaces

A Boolean indicating that the surfaces of up to target faces should be extended before extending and trimming the selected faces. The default value is True.

upToReferenceRep

A Boolean indicating that the selected faces should be extended along the selected edges and be trimmed along their intersection with the reference representation.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

FaceFromElementFaces(elementFaces: Region, stitch: BooleanType = 0, stitchTolerance: float | None = None, analyticFitTolerance: float | None = None, associateFace: BooleanType = 0)

This method creates a geometry face from a collection of orphan element faces.

Parameters:

elementFaces

A Region object specifying the collection of orphan element faces.

stitch

A Boolean specifying whether the created geometry face should be stitched with existing geometry faces. Default value is TRUE.

stitchTolerance

A Float indicating the maximum gap to be stitched. The value should be smaller than the minimum feature size and bigger than the maximum gap expected to be stitched in the model. Otherwise this command may remove small (sliver) edges that are smaller than the tolerance. If stitch tolerance is not provided then default value of 0.001 will be used for stitching.

analyticFitTolerance

A Float indicating the analytical surface fitting tolerance. If analytical tolerance is not provided then default value of 0.015 will be used for analytical surface fitting.

associateFace

A Boolean specifying whether the created geometry face should be associated with the mesh. Default value is TRUE.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

HoleBlindFromEdges(plane: str, planeSide: SymbolicConstantType, diameter: float, edge1: Edge, distance1: float, edge2: Edge, distance2: float, depth: float)

This method creates an additional Feature object by creating a circular blind hole of the given diameter and depth and cutting away material in the solid and shell regions of the part. The center of the hole is offset from two non-parallel straight edges by the given distances.

Parameters:

plane

A Datum plane object or a planar Face object.

planeSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

diameter

A Float specifying the diameter of the hole.

edge1

An Edge object specifying the edge from which distance1 is measured.

distance1

A Float specifying the offset from edge1.

edge2

An Edge object specifying the edge from which distance2 is measured.

distance2

A Float specifying the offset from edge2.

depth

A Float specifying the depth of the hole.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

HoleFromEdges(diameter: float, edge1: Edge, distance1: float, edge2: Edge, distance2: float)

This method creates an additional Feature object by creating a circular hole of the given diameter in a 2D planar part and cutting away material in the shell and wire regions of the part. The center of the hole is offset from two non-parallel straight edges by the given distances.

Parameters:

diameter

A Float specifying the diameter of the hole.

edge1

An Edge object specifying the edge from which distance1 is measured.

distance1

A Float specifying the offset from edge1.

edge2

An Edge object specifying the edge from which distance2 is measured.

distance2

A Float specifying the offset from edge2.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

HoleThruAllFromEdges(plane: str, planeSide: SymbolicConstantType, diameter: float, edge1: Edge, distance1: float, edge2: Edge, distance2: float)

This method creates an additional Feature object by creating a circular through hole of the given diameter and cutting away material in the solid and shell regions of the part. The center of the hole is offset from two non-parallel straight edges by the given distances.

Parameters:

plane

A Datum plane object or a planar Face object.

planeSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

diameter

A Float specifying the diameter of the hole.

edge1

An Edge object specifying the edge from which distance1 is measured.

distance1

A Float specifying the offset from edge1.

edge2

An Edge object specifying the edge from which distance2 is measured.

distance2

A Float specifying the offset from edge2.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Lock()

This method locks the part. Locking the part prevents any further changes to the part that can trigger regeneration of the part.

LockForUpgrade()

This method locks the part for upgrade. Locking the part prevents any further changes to the part that can trigger regeneration of the part. When the part is unlocked, all the parts are upgraded and regenrated.

MakeSketchTransform(sketchPlane: str, origin: tuple = (), sketchOrientation: SymbolicConstantType = 'RIGHT', sketchPlaneSide: SymbolicConstantType = 'SIDE1', sketchUpEdge: str = '')

This method creates a Transform object. A Transform object is a 4x3 matrix of Floats that represents the transformation from sketch coordinates to part coordinates.

Parameters:

sketchPlane

A Datum plane object or a planar Face object specifying the sketch plane.

origin

A sequence of Floats specifying the X-, Y-, and Z-coordinates that will be used as the origin of the sketch. The default value is computed as the centroid of the face.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

sketchPlaneSide

A SymbolicConstant specifying on which side of the sketchPlane the sketch is positioned. Possible values are SIDE1 and SIDE2. The default value is SIDE1.

sketchUpEdge

An Edge or DatumAxis object specifying the orientation of the sketch. If unspecified, the sketch is assumed to be oriented with the Y-direction pointing up.

Returns:

A Transform object. A Transform is an object with one method that returns the transform

matrix.

Raises:

• If the sketchUpEdge is parallel to the sketchPlane:

  Up direction is parallel to plane normal

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

MaterialOrientation(region: ~abaqus.Region.Set.Set | None = None, localCsys: ~abaqus.Datum.DatumCsys.DatumCsys = <abaqus.Datum.DatumCsys.DatumCsys object>, axis: ~abaqusConstants.SymbolicConstantType = 'AXIS_1', angle: float = 0, stackDirection: ~abaqusConstants.SymbolicConstantType = 'STACK_3', fieldName: str = '', orientationType: ~abaqusConstants.SymbolicConstantType = 'GLOBAL', normalAxisDirection: ~abaqusConstants.SymbolicConstantType = 'AXIS_3', normalAxisDefinition: ~abaqusConstants.SymbolicConstantType = 'NORMAL_VECTOR', normalAxisRegion: ~abaqus.Region.Surface.Surface | None = None, normalAxisDatum: ~abaqus.Datum.DatumAxis.DatumAxis = <abaqus.Datum.DatumAxis.DatumAxis object>, flipNormalDirection: ~abaqusConstants.BooleanType = 0, normalAxisVector: tuple = (), primaryAxisDirection: ~abaqusConstants.SymbolicConstantType = 'AXIS_1', primaryAxisDefinition: ~abaqusConstants.SymbolicConstantType = 'PRIMARY_VECTOR', primaryAxisRegion: ~abaqus.Region.Set.Set | None = None, primaryAxisDatum: ~abaqus.Datum.DatumAxis.DatumAxis = <abaqus.Datum.DatumAxis.DatumAxis object>, flipPrimaryDirection: ~abaqusConstants.BooleanType = 0, primaryAxisVector: tuple = ()) → MaterialOrientation

This method creates a MaterialOrientation object.

Parameters:

region

A Set object specifying a region for which the material orientation is defined.

localCsys

A DatumCsys object specifying the local coordinate system or None, describing the material orientation for the given region. In the ODB, this member was previously accessible using “csys,” but support has now been added for localCsys and the csys member will be deprecated.

axis

A SymbolicConstant specifying the axis of a datum coordinate system about which an additional rotation is applied. For shells this axis is also the shell normal. Possible values are AXIS_1, AXIS_2, and AXIS_3. The default value is AXIS_1.

angle

A Float specifying the angle of the additional rotation (if accessed from the ODB instead of the MDB, it will be a string instead of a float). The default value is 0.0.

stackDirection

A SymbolicConstant specifying the stack or thickness direction. Possible values are STACK_1, STACK_2, STACK_3, and STACK_ORIENTATION. The default value is STACK_3.

fieldName

A String specifying the name of the DiscreteField object specifying the orientation. The default value is an empty string.

orientationType

A SymbolicConstant specifying the method used to define the material orientation. If orientationType*=SYSTEM, the *region and localCsys arguments are required. If orientationType*=FIELD, the *fieldName argument is required. Possible values are GLOBAL, SYSTEM, FIELD, DISCRETE, and USER. The default value is GLOBAL.

normalAxisDirection

A SymbolicConstant specifying the axis that is defined by the normal axis direction for a discrete orientation. Possible values are AXIS_1, AXIS_2, and AXIS_3. The default value is AXIS_3.

normalAxisDefinition

A SymbolicConstant specifying the method used to define the normal axis direction for a discrete orientation. Possible values are SURFACE, NORMAL_DATUM, and NORMAL_VECTOR. The default value is NORMAL_VECTOR.

normalAxisRegion

A Surface object specifying a region whose geometric normals define the normal axis for the discrete orientation.

normalAxisDatum

A DatumAxis object specifying the Datum Axis or None, describing the normal axis direction for the discrete orientation.

flipNormalDirection

A Boolean specifying the flag to reverse the direction of the defined normal axis direction. The default value is OFF.

normalAxisVector

A sequence of Floats specifying the vector that defines the direction of the normal axis of the discrete orientation.

primaryAxisDirection

A SymbolicConstant specifying the axis that is defined by the primary axis direction for a discrete orientation. Possible values are AXIS_1, AXIS_2, and AXIS_3. The default value is AXIS_1.

primaryAxisDefinition

A SymbolicConstant specifying the method used to define the primary axis direction for a discrete orientation. Possible values are SURFACE, PRIMARY_DATUM, and PRIMARY_VECTOR. The default value is PRIMARY_VECTOR.

primaryAxisRegion

A Set object specifying a region whose geometric tangents define the primary axis for the discrete orientation.

primaryAxisDatum

A DatumAxis object specifying the Datum Axis or None, describing the primary axis direction for the discrete orientation.

flipPrimaryDirection

A Boolean specifying the flag to reverse the direction of the defined primary axis direction. The default value is OFF.

primaryAxisVector

A sequence of Floats specifying the vector that defines the direction of the primary axis of the discrete orientation.

Returns:

orientation: MaterialOrientation

A MaterialOrientation object.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].MaterialOrientation

MergeEdges(edgeList: tuple[Edge] = (), extendSelection: BooleanType = 0)

This method merges edges either by extending the user selection or using only the selected edges.

Parameters:

edgeList

A sequence of Edge objects specifying the edges to be merged.

extendSelection

A Boolean specifying whether the user selection needs to be extended to include edges till branching occurs. Branching is said to occur when the vertex of an edge is shared by more than two edges.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Mirror(mirrorPlane: str, keepOriginal: BooleanType, keepInternalBoundaries: BooleanType = 0)

This method mirrors existing part geometry across a plane to create new geometry.

Parameters:

mirrorPlane

A Datum plane object or a planar Face object.

keepOriginal

A boolean specifying whether or not the original part geometry should be retained.

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Node(coordinates: tuple, localCsys: ~abaqus.Datum.DatumCsys.DatumCsys = <abaqus.Datum.DatumCsys.DatumCsys object>, label: int | None = None)

This method creates a node on an orphan mesh part.

Parameters:

coordinates

A sequence of three Floats specifying the coordinates of the new node.

localCsys

A DatumCsys object specifying the local coordinate system. If unspecified, the global coordinate system will be used.

label

An Int specifying the node label.

Returns:

A MeshNode object.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].Node

OffsetFaces(faceList: tuple[Face], distance: float | None = None, targetFaces: tuple[Face] = (), targetFacesMethod: SymbolicConstantType | None = None, fractionDistance: float | None = None, trimToReferenceRep: BooleanType = 0)

This method creates new faces by offsetting existing faces.

Parameters:

faceList

A sequence of Face objects specifying the faces that will be offset. The faces may belong to the part or to the reference representation associated with the part.

distance

A Float indicating the distance to offset the faces. Either distance or targetFaces must be specified.

targetFaces

A sequence of Face objects whose distance to the faces argument together with the targetFacesMethod determines the distance to offset the faces. Either distance or targetFaces must be specified.

targetFacesMethod

A SymbolicConstant indicating how to calculate the distance to offset. It can have one of the following values:HALF_OF_AVERAGE: Offset the faces by a distance equals to half the average distance to target faces.CLOSEST_POINT_FRACTION: Offset the faces by a distance equals to the fraction of the distance to the approximate closest point on the selected target faces.FARTHEST_POINT_FRACTION: Offset the faces by a distance equals to the fraction of the distance to the approximate farthest point on the selected target faces.

fractionDistance

A Float indicating the fraction of the distance to the closest or the farthest point on the target faces. Its default value is 0.5.

trimToReferenceRep

A Boolean indicating whether to extend the offset faces and trim them along their intersection with the reference representation.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Part2DGeomFrom2DMesh(name: str, part: PartBase, featureAngle: float, splineCurvatureLimit: float = 90, twist: BooleanType = 0)

This method creates a geometric Part object from the outline of an existing two-dimensional orphan mesh Part object and places it in the parts repository. If the Part2DGeomFrom2DMesh method cannot create a valid two-dimensional shell section from the two-dimensional mesh, the method fails and creates an empty geometry part with a failed base shell feature.

Parameters:

name

A String specifying the repository key.

part

A Part object specifying an existing two-dimensional orphan mesh Part object.

featureAngle

A Float specifying the angle (in degrees) between line segments that triggers a break in the geometry.

splineCurvatureLimit

A Float specifying the traversal angle in degrees of the spline that triggers a break in the geometry. The default value is 90.

twist

A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when *dimensionality*=AXISYMMETRIC and *type*=DEFORMABLE_BODY). The default value is OFF.

Returns:

part: Part

A Part object If the specified part is not an orphan mesh part:

Specified part must be an orphan mesh.

If the Part2DGeomFrom2DMesh method cannot create a valid two-dimensional shell section from the two-dimensional mesh:

Planar shell feature failed

If the specified part is not two-dimensional:

Cannot create a geometry from a 3D part.

If the specified part is a rigid body:

Cannot create a geometry from a rigid body.

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromBooleanCut(name: str, instanceToBeCut: str, cuttingInstances: tuple[abaqus.Part.PartBase.PartInstance])

This method creates a Part in the parts repository after subtracting or cutting the geometries of a group of part instances from that of a base part instance.

Parameters:

name

A String specifying the repository key.

instanceToBeCut

A PartInstance specifying the base instance from which to cut other instances.

cuttingInstances

A sequence of PartInstance objects specifying the instances with which to cut the base instance.

Returns:

part: Part

A Part object

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromBooleanMerge(name: str, instances: tuple[abaqus.Part.PartBase.PartInstance], keepIntersections: BooleanType = False, mergeNodes: SymbolicConstantType = 'BOUNDARY_ONLY', nodeMergingTolerance: float | None = None, removeDuplicateElements: BooleanType = 1, domain: SymbolicConstantType = 'GEOMETRY')

This method creates a Part in the parts repository after merging two or more part instances. The part instances can be either Abaqus native parts or orphan mesh parts, but they cannot be a combination of both.

Parameters:

name

A String specifying the repository key.

instances

A sequence of PartInstance objects specifying the part instances to merge.

keepIntersections

A Boolean specifying whether the boundary intersections of Abaqus native part instances should be retained after the merge operation. The default value is False.

mergeNodes

A SymbolicConstant specifying whether the nodes of orphan mesh part instances should be retained after the merge operation. Possible values are BOUNDARY_ONLY, ALL, or NONE. The default value is BOUNDARY_ONLY.

nodeMergingTolerance

A Float specifying the maximum distance between nodes of orphan mesh part instances that will be merged and replaced with a single new node. The location of the new node is the average position of the deleted nodes. The default value is 10–6.

removeDuplicateElements

A Boolean specifying whether elements with the same connectivity after the merge will merged into a single element. The default value is ON.

domain

A SymbolicConstant specifying whether the part instances being merged are geometric instances or mesh instances. Possible values are GEOMETRY, MESH or BOTH. The default value is GEOMETRY.

Returns:

part: Part

A Part object

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromExtrude2DMesh(name: str, part: PartBase, depth: float, elementSize: float)

This method creates a Part object by extruding an existing two-dimensional orphan mesh Part object in the positive Z-direction and places it in the parts repository.

Parameters:

name

A String specifying the repository key.

part

A Part object specifying an existing two-dimensional orphan mesh Part object.

depth

A Float specifying the total extrusion distance.

elementSize

A Float specifying an approximate element length in the extruded direction.

Returns:

part: Part

A Part object - If the specified part is not an orphan mesh part:

Cannot extrude a geometric part.

• If the specified part is not two-dimensional: Cannot extrude a 3D part.

• If the specified part is a rigid body: Cannot change dimension of a rigid body.

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromGeometryFile(name: str, geometryFile: AcisFile, dimensionality: SymbolicConstantType, type: SymbolicConstantType, bodyNum: int = 1, combine: BooleanType = False, booleanSolids: BooleanType = False, retainBoundary: BooleanType = False, usePartNameFromFile: BooleanType = 0, stitchTolerance: float = 1, twist: BooleanType = 0, scale: float = 1, convertToAnalytical: int = 0, convertToPrecise: int = 0)

This method creates a Part object and places it in the parts repository.

Parameters:

name

A String specifying the repository key.

geometryFile

An AcisFile object specifying a file containing geometry.

dimensionality

A SymbolicConstant specifying the dimensionality of the part. Possible values are THREE_D, TWO_D_PLANAR, and AXISYMMETRIC.

type

A SymbolicConstant specifying the type of the part. Possible values are DEFORMABLE_BODY, EULERIAN, DISCRETE_RIGID_SURFACE, and ANALYTIC_RIGID_SURFACE.

bodyNum

An Int specifying the desired body to be selected from an ACIS object containing a list of N ACIS bodies. Possible values are 1 ≤≤ bodyNum ≤≤ N. The default value is 1.

combine

A Boolean specifying weather to create a single part by combining all the bodies in the ACIS object. This argument is ignored if bodyNum is specified. The default value is False.

booleanSolids

A Boolean specifying whether the solids should be boolean while combining all the bodies.The default value is FALSE.

retainBoundary

A Boolean specifying whether the intersecting boundaries should be retained while boolean the solids.The default value is FALSE.

usePartNameFromFile

A Boolean specifying whether the part names specified in a STEP file should be used as the names in the Abaqus model database. If this option is TRUE, the part names in the STEP file will be used; if FALSE, each imported part will be named using the text of the name argument followed by a number. This functionality is available only for import from STEP files; for import from all other types of files this option should be FALSE.

stitchTolerance

A Float indicating the maximum gap to be stitched. The value should be smaller than the minimum feature size and bigger than the maximum gap expected to be stitched in the model. Otherwise this command may remove small (sliver) edges that are smaller than the tolerance. The default value is 1.0

twist

A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when *dimensionality*=AXISYMMETRIC and *type*=DEFORMABLE_BODY). The default value is OFF.

scale

A Float specifying the scaling factor to apply to the imported geometric entities. The default value is 1.0.

convertToAnalytical

An Int specifying whether to convert to analytical entities. Possible values are 0 or 1. The default value is 0. If *convertToAnalytical*=1, all the numerical entities, such as splines, are converted to analytical entities, such as arcs and lines, during the repair phase of the command.

convertToPrecise

An Int specifying whether to convert to precise geometry. Possible value are 0 or 1. The default value is 0. If *convertToPrecise*=1, the application will attempt to re-evaluate the tolerant entities to be more precise.

Returns:

part: Part

A Part object - If the ACIS file is corrupt:

PartError: the file is corrupt

• If the dimensionality does not correspond to what is found in the ACIS file: PartError: dimensionality does not match the contents of the file

• If the type does not correspond to what is found in the ACIS file: PartError: type does not match the contents of the file

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromInstanceMesh(name: str, partInstances: tuple[abaqus.Part.PartBase.PartInstance] = (), copyPartSets: BooleanType = False, copyAssemblySets: BooleanType = False)

This method creates a Part object containing the mesh found in the supplied PartInstance objects and places the new Part object in the parts repository.

Parameters:

name

A String specifying the repository key.

partInstances

A sequence of PartInstance objects to be used in the creation of the new mesh part. If the partInstances argument is omitted, the new Part object contains the mesh of all the part instances in the assembly.

copyPartSets

A Boolean specifying whether to copy sets, surfaces, and attributes from the base part or parts of the specified part instances to the new part. The default is False.

copyAssemblySets

A Boolean specifying whether to copy assembly-level sets that reference entities of the specified part instances to the new part. The default is False.

Returns:

part: Part

A Part object - If the analysis type (deformable or rigid) is not consistent among the supplied part instances:

The selected part instances do not have a consistent analysis type.

• If the assembly does not contain a mesh: The current assembly does not contain a mesh for a mesh part.

• If the specified part instances do not contain a mesh: The selected part instances do not have a mesh for a mesh part.

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromMesh(name: str, copySets: BooleanType = False)

This method creates a Part object containing the mesh found in the part and places the new Part object in the parts repository.

Parameters:

name

A String specifying the repository key.

copySets

A Boolean specifying whether to copy sets, surfaces, and attributes to the new part. The default is False.

Returns:

part: Part

A Part object - If the part does not contain a mesh:

The current part does not contain a mesh for a mesh part.

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromMeshMirror(name: str, part: PartBase, point1: tuple, point2: tuple)

This method creates a Part object by mirroring an existing orphan mesh Part object about a specified plane and places it in the parts repository. The result is a union of the original and the mirrored copy. Contrast the PartFromMeshMirror method with the mirrorPlane argument of the Part copy constructor. The mirrorPlane argument creates only the second half of the part but does not unite the two halves.

Parameters:

name

A String specifying the repository key.

part

A Part object specifying an existing orphan mesh part.

point1

A sequence of three Floats specifying a point on the mirror plane. This point is the local origin in the local system of the plane.

point2

A sequence of three Floats specifying a point in the direction of the normal to the mirror plane. This point must not be coincident with point1.

Returns:

part: Part

A Part object - If the specified part is not an orphan mesh part:

Cannot mirror a geometric part.

• If the specified part is a rigid body: Cannot mirror a rigid body.

• If point1 and point2 are coincident: Mirror plane director has zero length.

• If the specified part is two-dimensional and the plane is not parallel to the

Z-axis:

Mirror plane must be parallel to Z axis for 2D parts

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromNodesAndElements(name: str, dimensionality: SymbolicConstantType, type: SymbolicConstantType, nodes: tuple, elements: tuple, twist: BooleanType = 0)

This method creates a Part object from nodes and elements and places it in the parts repository.

Parameters:

name

A String specifying the repository key.

dimensionality

A SymbolicConstant specifying the dimensionality of the part. Possible values are THREE_D, TWO_D_PLANAR, and AXISYMMETRIC.

type

A SymbolicConstant specifying the type of the part. Possible values are DEFORMABLE_BODY, EULERIAN, DISCRETE_RIGID_SURFACE, and ANALYTIC_RIGID_SURFACE.

nodes

A sequence of (nodeLabels, nodeCoords) specifying the nodes of the mesh. nodeLabels is a sequence of Ints specifying the node labels, and nodeCoords is a sequence of sequences of three Floats specifying the nodal coordinates.

elements

A sequence of sequences of(meshType, elementLabels, elementConns) specifying the elements of the mesh. meshType is a String specifying the element type. elementlabels is a sequence of Ints specifying the element labels. elementConns is a sequence of sequences of node labels specifying the element connectivity.

twist

A boolean specifying whether the part is defined with twist. This option has meaning only when *dimensionality*=AXISYMMETRIC. Possible values are ON and OFF. The default value is OFF.

Returns:

part: Part

A Part object

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromOdb(name: str, odb: str, fileName: str = '', instance: str = '', elementSet: str = '', shape: SymbolicConstantType = 'UNDEFORMED', step: int | None = None, frame: int | None = None, twist: BooleanType = 0)

This method creates an orphan mesh Part object by reading an output database. The new part is placed in the parts repository.

Parameters:

name

A String specifying the repository key.

odb

An output database object.

fileName

A String specifying the name of the output database file from which to create the part. The default value is an empty string.

instance

A String specifying the part instance in the output database from which to create the part. If no instance name is specified, Abaqus creates an orphan mesh part from the first part instance in the output database.

elementSet

A String specifying an element set defined on the output database. Only elements from this set will be imported. The default is to import all element sets.

shape

A SymbolicConstant specifying the configuration state. Possible values are UNDEFORMED and DEFORMED. The default value is UNDEFORMED.

step

An Int specifying the step number for reading deformed coordinates. 0≤step≤N−10≤step≤N-1 where NN is the number of available steps. The default value is the last available step. You should specify the step argument only when *shape*=DEFORMED.

frame

An Int specifying the frame number for reading deformed coordinates. 0≤frame≤N−10≤frame≤N-1 where NN is the number of available frames. The default value is the last available frame. You should specify the frame argument only when *shape*=DEFORMED.

twist

A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when *dimensionality*=AXISYMMETRIC and *type*=DEFORMABLE_BODY). The default value is OFF.

Returns:

part: Part

A Part object - If the output database contains elements of more than one dimensionality or type:

File contains both axisymmetric and nonaxisymmetric elements.File contains both 2D and

3D elements.File contains both rigid and deformable elements. - If more than one part is found on the output database:

PartError: importing of more than one part is not currently supported

• If the output database does not contain any valid results for the specified step: Error. File does not contain any valid frames.

• If the specified step and frame do not contain any displacements: Error. Specified frame does not contain nodal displacements.

• If the specified element set is not found on the output database: Error. Specified element set is not defined in the ODB.

• If the step number is invalid: OdiError: Invalid step index: i. Available step indices: 0 - j.

• If the frame number is invalid: OdiError: Invalid frame index: i. Available frame indices: 0 - j.

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromSection3DMeshByPlane(name: str, part: PartBase, point1: float, point2: float, point3: tuple)

This method creates a Part object by cutting an existing three-dimensional orphan mesh Part object by a plane and places it in the parts repository. This method is valid only for orphan mesh parts composed of 8-node brick elements.

Parameters:

name

A String specifying the repository key.

part

A Part object specifying an existing three-dimensional orphan mesh part.

point1

A Sequence of three Floats specifying a point on the cutting plane. This point is the local origin in the local system of the plane.

point2

A Sequence of three Floats specifying a point in the direction of the normal to the cutting plane. This point must not be coincident with point1.

point3

A sequence of three Floats specifying the direction of the local 1-axis in the local system of the plane. This point must not project onto point1.

Returns:

part: Part

A Part object - If the specified part is not an orphan mesh part:

Cannot reduce dimension of a geometric part.

• If the specified part is not three-dimensional: Cannot reduce dimension of a 2D part.

• If the specified part is a rigid body: Cannot change dimension of a rigid body.

• If point1 and point2 are coincident: Cutting plane director has zero length.

• If point3 projects onto point1: Local axis point projects to origin.

• If no elements are cut by the specified plane: Cannot reduce part dimension.

Notes

This function can be accessed by:

mdb.models[name].Part

PartFromSubstructure(name: str, substructureFile: str, odbFile: str)

This method creates a substructure Part object by reading a substructure sim file and places it in the parts repository.

Parameters:

name

A String specifying the repository key.

substructureFile

A substructure sim file.

odbFile

The output database file corresponding to the substructure sim file.

Returns:

part: Part

A Part object - If the specified part is not a substructure:

File specified does not contain a substructure.

• If the specified part already exists: A part with the same name already exists.

• If the substructure cannot be imported: The output database is missing nodes and elements.Nested substructures are not

supported.The substructure sim file was generated using a version that is different from the current version.

Notes

This function can be accessed by:

mdb.models[name].Part

PartitionCellByDatumPlane(cells: tuple[Cell], datumPlane: DatumPlane)

This method partitions one or more cells using the given datum plane.

Parameters:

cells

A sequence of Cell objects specifying the cells to partition.

datumPlane

A DatumPlane object.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionCellByExtendFace(cells: tuple[Cell], extendFace: str)

This method partitions one or more cells by extending the underlying geometry of a given face to partition the target cells.

Parameters:

cells

A sequence of Cell objects specifying the cells to partition.

extendFace

A planar, cylindrical, conical, or spherical Face object.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionCellByExtrudeEdge(cells: tuple[Cell], edges: str, line: str, sense: SymbolicConstantType)

This method partitions one or more cells by extruding selected edges in the given direction.

Parameters:

cells

A sequence of Cell objects specifying the cells to partition.

edges

The Edge objects to be extruded. The edges must be in the same plane. The edges must form a continuous chain, without branches. The edges must belong to the same PartInstance object.

line

A straight Edge or DatumAxis object specifying the extrude direction. line must be perpendicular to the plane formed by edges.

sense

A SymbolicConstant specifying the direction of the extrusion. Possible values are FORWARD and REVERSE. If sense*=FORWARD, the extrusion is in the direction of *line.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionCellByPatchNCorners(cell: Cell, cornerPoints: tuple)

This method partitions a cell using an N-sided cutting patch defined by the given corner points.

Parameters:

cell

A Cell object specifying the cell to partition.

cornerPoints

A sequence of ConstrainedSketchVertex, InterestingPoint, or DatumPoint objects. 3 ≤≤ len(cornerPoints) ≤≤ 5. The corner points must not coincide.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionCellByPatchNEdges(cell: str, edges: tuple[Edge])

This method partitions a cell using an N-sided cutting patch defined by the given edges.

Parameters:

cell

A Cell specifying the cell to partition.

edges

A sequence of Edge objects bounding the patch. The edges must form a closed loop. The Edge objects must belong to the same PartInstance object as cell.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionCellByPlaneNormalToEdge(cells: tuple[Cell], edge: Edge, point: int)

This method partitions one or more cells using a plane normal to an edge at the given edge point.

Parameters:

cells

A sequence of Cell objects specifying the cells to partition.

edge

An Edge object specifying the normal to the plane.

point

A ConstrainedSketchVertex, InterestingPoint, or DatumPoint object specifying a point on edge.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionCellByPlanePointNormal(cells: tuple[Cell], point: int, normal: str)

This method partitions one or more cells using a plane defined by a point and a normal direction.

Parameters:

cells

A sequence of Cell objects specifying the cells to partition.

point

A ConstrainedSketchVertex, InterestingPoint, or DatumPoint object specifying a point on the plane.

normal

A straight Edge or DatumAxis object specifying the normal to the plane.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionCellByPlaneThreePoints(cells: tuple[Cell], point1: int, point2: int, point3: int)

This method partitions one or more cells using a plane defined by three points.

Parameters:

cells

A sequence of Cell objects specifying the cells to partition.

point1

A ConstrainedSketchVertex, InterestingPoint, or DatumPoint object specifying a point on the plane.

point2

A ConstrainedSketchVertex, InterestingPoint, or DatumPoint object specifying a point on the plane.

point3

A ConstrainedSketchVertex, InterestingPoint, or DatumPoint object specifying a point on the plane.Note:point1, point2, and point3 must not be colinear and must not coincide.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionCellBySweepEdge(cells: tuple[Cell], edges: tuple[Edge], sweepPath: Edge)

This method partitions one or more cells by sweeping selected edges along the given sweep path.

Parameters:

cells

A sequence of Cell objects specifying the cells to partition.

edges

A sequence of Edge objects to be swept. The edges must be in the same plane. The edges must form a continuous chain without branches. The Edge objects must all belong to the same PartInstance object.

sweepPath

An Edge object specifying the sweep path. The start of sweepPath must be in the plane and perpendicular to the plane formed by edges. The sweep path must be planar.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionEdgeByDatumPlane(edges: tuple[Edge], datumPlane: DatumPlane)

This method partitions an edge where it intersects with a datum plane.

Parameters:

edges

A sequence of Edge objects specifying the edges to partition.

datumPlane

A DatumPlane object specifying the location of the partition.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionEdgeByParam(edges: tuple[Edge], parameter: float)

This method partitions one or more edges at the given normalized edge parameter.

Parameters:

edges

A sequence of Edge objects specifying the edges to partition.

parameter

A Float specifying the normalized distance along edge at which to partition. Possible values are 0.0 << parameter << 1.0.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionEdgeByPoint(edge: Edge, point: int)

This method partitions an edge at the given point.

Parameters:

edge

An Edge object specifying the edge to partition.

point

An InterestingPoint or DatumPoint object specifying a point on edge.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionFaceByAuto(face: Face)

This method automatically partitions a target face into simple regions that can be meshed using a structured meshing technique.

Parameters:

face

A Face object specifying the face to partition.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionFaceByCurvedPathEdgeParams(face: Face, edge1: Edge, parameter1: float, edge2: Edge, parameter2: float)

This method partitions a face normal to two edges, using a curved path between the two given edge points defined by the normalized edge parameters.

Parameters:

face

A Face object specifying the face to partition.

edge1

An Edge object specifying the start of the partition. The edge must belong to face.

parameter1

A Float specifying the distance along edge1 at which to partition. Possible values are 0.0 ≤≤ distance1 ≤≤ 1.0.

edge2

An Edge object specifying the end of the partition. The edge must belong to face.

parameter2

A Float specifying the distance along edge2 at which to partition. Possible values are 0.0 ≤≤ distance2 ≤≤ 1.0.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionFaceByCurvedPathEdgePoints(face: Face, edge1: Edge, point1: int, edge2: Edge, point2: int)

This method partitions a face normal to two edges, using a curved path between the two given edge points.

Parameters:

face

A Face object specifying the face to partition.

edge1

An Edge object specifying the start of the partition. The edge must belong to face.

point1

A ConstrainedSketchVertex, InterestingPoint, or DatumPoint object specifying a point on edge1.

edge2

An Edge object specifying the end of the partition. The edge must belong to face.

point2

A ConstrainedSketchVertex, InterestingPoint, or DatumPoint object specifying a point on edge2.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionFaceByDatumPlane(faces: tuple[Face], datumPlane: DatumPlane)

This method partitions one or more faces using the given datum plane.

Parameters:

faces

A sequence of Face objects specifying the faces to partition.

datumPlane

A DatumPlane object specifying the location of the partition.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionFaceByExtendFace(faces: tuple[Face], extendFace: Face)

This method partitions one or more faces by extending the underlying geometry of another given face to partition the target faces.

Parameters:

faces

A sequence of Face objects specifying the faces to partition.

extendFace

A Face object that is to be extended to create the partition. The face to extend can be a planar, cylindrical, conical, or spherical face.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionFaceByIntersectFace(faces: tuple[Face], cuttingFaces: tuple[Face])

This method partitions one or more faces using the given cutting faces to partition the target faces.

Parameters:

faces

A sequence of Face objects specifying the faces to partition.

cuttingFaces

A sequence of Face objects that specify the cutting faces.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionFaceByProjectingEdges(faces: tuple[Face], edges: tuple[Edge], extendEdges: BooleanType = False)

This method partitions one or more faces by projecting the given edges on the target faces.

Parameters:

faces

A sequence of Face objects specifying the faces to partition.

edges

A sequence of Edge objects specifying the edges that will be projected onto the target faces.

extendEdges

A boolean specifying whether to extend the given edges at their free ends in the tangent direction before partitioning the target faces. The default value is False.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionFaceByShortestPath(faces: tuple[Face], point1: int, point2: int)

This method partitions one or more faces using a minimum distance path between the two given points.

Parameters:

faces

A sequence of Face objects specifying the face to partition.

point1

A ConstrainedSketchVertex, InterestingPoint, or DatumPoint object.

point2

A ConstrainedSketchVertex, InterestingPoint, or DatumPoint object.Note:point1 and point2 must not coincide, and they must both lie on the underlying surface geometry of at least one of the target faces.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionFaceBySketch(faces: tuple[Face], sketch: ConstrainedSketch, sketchUpEdge: str = '', sketchOrientation: SymbolicConstantType = 'RIGHT')

This method partitions one or more planar faces by sketching on them.

Parameters:

faces

A sequence of Face objects specifying the faces to partition.

sketch

A ConstrainedSketch object specifying the partition.

sketchUpEdge

An Edge or DatumAxis object specifying the orientation of sketch. This edge or datum axis must not be orthogonal to the plane defined by faces. If unspecified, sketch is assumed to be oriented in with the Y direction pointing up.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionFaceBySketchDistance(faces: tuple[Face], sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, distance: float, sketchOrientation: SymbolicConstantType = 'RIGHT')

This method partitions one or more faces by sketching on a sketch plane and then projecting the sketch toward the target faces through the given distance.

Parameters:

faces

A sequence of Face objects specifying the faces to partition.

sketchPlane

A planar Face or DatumPlane object.

sketchPlaneSide

A SymbolicConstant specifying the side of the plane to be used for sketching. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object specifying the orientation of sketch. This edge must not be orthogonal to sketchPlane.

sketch

A ConstrainedSketch object specifying the partition.

distance

A Float specifying the projection distance. Possible values are distance >> 0.0.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionFaceBySketchRefPoint(faces: tuple[Face], sketchPlane: str, sketchUpEdge: Edge, sketch: ConstrainedSketch, point: int, sketchOrientation: SymbolicConstantType = 'RIGHT')

This method partitions one or more faces by sketching on a sketch plane and then projecting the sketch toward the target faces through a distance governed by the reference point.

Parameters:

faces

A sequence of Face objects specifying the faces to partition.

sketchPlane

A planar Face or DatumPlane object.

sketchUpEdge

An Edge object or a DatumAxis object specifying the orientation of sketch. This edge or datum axis must not be orthogonal to sketchPlane.

sketch

A ConstrainedSketch object specifying the partition.

point

A ConstrainedSketchVertex, InterestingPoint, or DatumPoint object specifying the distance to project sketch. The point must not lie on sketchPlane.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

PartitionFaceBySketchThruAll(faces: tuple[Face], sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: str, sketch: ConstrainedSketch, sketchOrientation: SymbolicConstantType = 'RIGHT')

This method partitions one or more faces by sketching on a sketch plane and then projecting toward the target faces through an infinite distance.

Parameters:

faces

A sequence of Face objects specifying the faces to partition.

sketchPlane

A planar Face or DatumPlane object.

sketchPlaneSide

A SymbolicConstant specifying the extrude direction of the sketch. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge or a DatumAxis object specifying the orientation of sketch. This edge or datum axis must not be orthogonal to sketchPlane.

sketch

A ConstrainedSketch object specifying the partition.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

Returns:

A Feature object.

Raises:

AbaqusException.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

ReferencePoint(point: tuple | Vertex | InterestingPoint | MeshNode | Datum, instanceName: str = '') → Feature

This method creates a Feature object and a ReferencePoint object at the specified location.

Parameters:

point

A ConstrainedSketchVertex, InterestingPoint, a MeshNode, or a Datum object specifying a reference point. point can also be a sequence of three Floats representing the X-, Y-, and Z-coordinates of the point.

instanceName

Used internally by the input file writer.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

RemoveCells(cellList: tuple[Cell])

This method converts a solid entity to a shell entity.

Parameters:

cellList

A sequence of Cell objects specifying the cells to remove.

Returns:

A Boolean value.

Raises:

• If the intended volume to be turned into a shell entity is not three-dimensional.

  Parterror: ConstrainedSketchGeometry that is not 3-dimensional does not contain cells.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RemoveFaces(faceList: tuple[Face], deleteCells: BooleanType = False)

This method removes faces from a solid entity or from a shell entity.

Parameters:

faceList

A sequence of Face objects specifying the faces to remove.

deleteCells

A Boolean specifying whether all cells are to be deleted when the faces are removed. The default value is False.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RemoveFacesAndStitch(faceList: tuple[Face])

This method removes faces from a solid entity and attempts to close the resulting gap by extending the neighboring faces of the solid.

Parameters:

faceList

A sequence of Face objects specifying the faces to remove.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RemoveRedundantEntities(vertexList: tuple[Vertex] = (), edgeList: tuple[Edge] = (), removeEdgeVertices: BooleanType = True)

This method removes redundant edges and vertices from a solid or a shell entity. One of the two arguments is required.

Parameters:

vertexList

A sequence of ConstrainedSketchVertex objects specifying the vertices to be removed.

edgeList

A sequence of Edge objects specifying the edges to be removed.

removeEdgeVertices

A Boolean specifying whether the vertices of the redundant edges need to be removed. The default is True.

Returns:

A Feature object.

Raises:

• If the selected entity is not a redundant entity.

  Parterror: None of the selected entities are redundant.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RemoveWireEdges(wireEdgeList: tuple[Edge])

This method removes wire edges.

Parameters:

wireEdgeList

A sequence of Edge objects specifying the edges to remove. Any specified edge that is not a wire edge will not be removed.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AttachmentPoints
mdb.models[name].rootAssembly.AttachmentPoints

RepairFaceNormals(faceList: tuple[Face] = ())

This method works on the entire part or a sequence of shell faces. When the entire part is selected, it aligns all the shell face normals, and inverts all of the solid faces’ normals if the solid was originally inside out. When a few shell faces are selected, it inverts the normals of the selected faces.

Parameters:

faceList

A sequence of Face objects.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RepairInvalidEdges(edgeList: tuple[Edge])

This method repairs invalid edges. It will always attempt to improve edges even if none of selected edges are initially invalid and may leave behind invalid edges that could not be repaired.

Parameters:

edgeList

A sequence of Edge objects.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RepairSliver(face: Face, point1: int, point2: int, toleranceChecks: BooleanType = True)

This method repairs the selected sliver from the selected face. The sliver area is specified using two points. A face partition is carried out at the specified points and the smaller of the two faces is removed.

Parameters:

face

A Face object specifying the face on which the sliver is located.

point1

A point specifying the location for partition creation. It can be a ConstrainedSketchVertex object, an Interesting Point or three coordinates specifying the point on an edge of the face.

point2

A point specifying the location for partition creation. It can be a ConstrainedSketchVertex object, an Interesting Point or three coordinates specifying the point on an edge of the face.

toleranceChecks

A Boolean specifying whether to use internal tolerance checks to restrict the size of the sliver face being removed. The default is True.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RepairSmallEdges(edgeList: tuple[Edge], toleranceChecks: BooleanType = True)

This method repairs small edges. This method will attempt to replace selected small edges with vertices and extend the adjacent faces and edges. This method might leave behind some small edges that cannot be removed.

Parameters:

edgeList

A sequence of Edge objects.

toleranceChecks

A Boolean specifying whether to use internal tolerance checks to restrict the size of the edges being removed. The default is True.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RepairSmallFaces(faceList: tuple[Face], toleranceChecks: BooleanType = True)

This method repairs small faces. It will attempt to replace the selected small faces with edges or vertices and extend the adjacent faces. This method might leave behind some small faces that cannot be removed.

Parameters:

faceList

A sequence of Face objects.

toleranceChecks

A Boolean specifying whether to use internal tolerance checks to restrict the size of the faces being removed. The default is True.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

ReplaceFaces(faceList: tuple[Face], stitch: BooleanType = True)

This method replaces the selected faces with a single face. If one single face is selected, that alone is replaced with a new face.

Parameters:

faceList

A sequence of Face objects to be replaced.

stitch

A Boolean specifying whether the newly created face needs to be stitched to the existing geometry. The default is True.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Round(radius: float, edgeList: tuple[Edge], vertexList: tuple[Vertex])

This method creates an additional Feature object by rounding (filleting) the given list of entities with the given radius.

Parameters:

radius

A Float specifying the radius of the fillets.

edgeList

A sequence of Edge objects. Solid and Shell edges of a part can be rounded. The operation will fail for non-manifold edges. The edgeList and vertexList arguments are mutually exclusive. One of them must be specified.

vertexList

A sequence of ConstrainedSketchVertex objects. Vertices that are connected to two wire edges can be rounded. The operation will fail for a vertex connected to a face. The edgeList and vertexList arguments are mutually exclusive. One of them must be specified.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

SectionAssignment(region: Set, sectionName: str, thicknessAssignment: SymbolicConstantType = 'FROM_SECTION', offset: float = 0, offsetType: SymbolicConstantType = 'SINGLE_VALUE', offsetField: str = '')

This method creates a SectionAssignment object.

Parameters:

region

A Set object specifying the region to which the section is assigned.

sectionName

A String specifying the name of the section.

thicknessAssignment

A SymbolicConstant specifying section thickness assignment method. Possible values are FROM_SECTION and FROM_GEOMETRY. The default value is FROM_SECTION.

offset

A Float specifying the offset of the shell section. The default value is 0.0.

offsetType

A SymbolicConstant specifying the method used to define the shell offset. If offsetType is set to OFFSET_FIELD the offsetField must have a value. Possible values are SINGLE_VALUE, MIDDLE_SURFACE, TOP_SURFACE, BOTTOM_SURFACE, FROM_GEOMETRY, and OFFSET_FIELD. The default value is SINGLE_VALUE.

offsetField

A String specifying the name of the field specifying the offset. The default value is “”.

Returns:

assignment: SectionAssignment

A SectionAssignment object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].SectionAssignment
mdb.models[name].rootAssembly.SectionAssignment

Set(name, *args, **kwargs) → _overload_dummy

This method creates a set from a sequence of objects in a model database.

Parameters:

name

Returns:

set: Set

A Set object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].Set
mdb.models[name].rootAssembly.Set

Shell(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, sketchOrientation: SymbolicConstantType = 'RIGHT')

This method creates an additional Feature object by creating a planar shell from the given ConstrainedSketch object. The ConstrainedSketch object must define a closed profile.

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketch

A ConstrainedSketch object specifying the planar shell.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

ShellExtrude(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, depth: float | None = None, upToFace: str = '', sketchOrientation: SymbolicConstantType = 'RIGHT', draftAngle: float | None = None, pitch: float | None = None, flipExtrudeDirection: BooleanType = 0, keepInternalBoundaries: BooleanType = 0)

This method creates an additional Feature object by extruding the given ConstrainedSketch object by the given depth, creating a shell protrusion. The ConstrainedSketch object can define either an open or closed profile.

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketch

A ConstrainedSketch object specifying the planar sketch to be extruded.

depth

A Float specifying the extrusion depth. The default is to not specify a depth. Either depth or upToFace must be used to define the extrusion depth.

upToFace

A Face specifying the face up to which to extrude. If upToFace is specified, the extrusion will be an up-to-face extrusion. The default is to not specify a face. Either depth or upToFace must be used to define the extrusion depth.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

flipExtrudeDirection

A Boolean specifying whether to override the direction of feature creation. If the value is OFF, it means use the direction defined by the sketchPlaneSide; if the value is ON, it means use the opposite direction to the one defined by sketchPlaneSide. The default value is OFF.

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

ShellLoft(loftsections: tuple, startCondition: SymbolicConstantType | None = None, endCondition: SymbolicConstantType | None = None, startTangent: float | None = None, startMagnitude: float | None = None, endTangent: float | None = None, endMagnitude: float | None = None, paths: tuple = (), globalSmoothing: BooleanType = 0, keepInternalBoundaries: BooleanType = 0)

This method creates an additional Feature object by lofting between the given sections and adding shell faces to the part. You define the sections using a sequence of edges from the part or an EdgeArray.

Parameters:

loftsections

A sequence of sequences of edges specifying the cross-sections to be lofted. Each outer sequence specifies a section through which the method will pass the loft feature. Each outer sequence can be defined as a sequence of edges or as an EdgeArray. The edges specifying a section must form a simple closed profile and must not contain multiple loops.

startCondition

A SymbolicConstant specifying the tangent direction at the start section of the loft feature. Possible values are NONE, NORMAL, RADIAL and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the startCondition argument in conjunction with the endCondition argument.

endCondition

A SymbolicConstant specifying the tangent direction at the end section of the loft feature. Possible values are NONE, NORMAL, RADIAL and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the endCondition argument in conjunction with the startCondition argument.

startTangent

A Float specifying the angle in degrees of the tangent with respect to the plane in which the start section lies. You must specify the startTangent argument if startCondition*=SPECIFIED. Possible values are 0.0 ≤≤ *startTangent ≤≤ 180.0.

startMagnitude

A Float specifying the magnitude of the startTangent. You must specify the startMagnitude argument if startCondition*=SPECIFIED. Possible values are 0.0 << *startMagnitude << 100.0.

endTangent

A Float specifying the angle in degrees of the tangent with respect to the plane in which the end section lies. You must specify the endTangent argument if startCondition*=SPECIFIED. Possible values are 0.0 ≤≤ *endTangent ≤≤ 180.0.

endMagnitude

A Float specifying the magnitude of the endTangent. This argument is to be used when the endCondition argument has the value SPECIFIED. Possible values are 0.0 << endMagnitude << 100.0.

paths

A sequence of sequences of edges that pass through each section in the loft feature. Each sequence specifies a path followed by the face or an edge created by a loft feature. Each path must start at the first section, end at the last section, and pass through each section. In addition, the order of the sequences must be the same as the order of the sections in the loftsections argument. Each path must not self-intersect and must be tangent continuous. In addition, the paths must not intersect each other. You cannot use the paths argument in conjunction with the startCondition and endCondition arguments.

globalSmoothing

A Boolean specifying whether each path defined in the paths argument is applied locally or globally.If the path is applied locally, its effect is felt only on faces created from the edges on the loftsections through which the paths pass through.If the path is applied globally, an averaging algorithm is applied over all the paths defined and is distributed over all the faces created.The default value is ON (globally).

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

ShellRevolve(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, angle: float, sketchOrientation: SymbolicConstantType = 'RIGHT', pitch: float | None = None, flipRevolveDirection: BooleanType = 0, flipPitchDirection: BooleanType = 0, moveSketchNormalToPath: BooleanType = 0, keepInternalBoundaries: BooleanType = 0)

This method creates an additional Feature object by revolving the given ConstrainedSketch object by the given angle, creating a shell protrusion. The ConstrainedSketch object can define either an open or closed profile and an axis of revolution. The axis is defined by a single construction line. For a description of the plane positioning arguments, see SolidExtrude.

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketch

A ConstrainedSketch object specifying the planar sketch to be revolved.

angle

A Float specifying the angle in degrees to be revolved.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤≤ pitch ≤≤ 105. The default value, 0, implies a normal revolve.

flipRevolveDirection

A Boolean specifying whether to override the direction of feature creation. If *flipRevolveDirection*=OFF, the default direction of revolution is used. If *flipRevolveDirection*=ON, the revolve direction is reversed. The default value is OFF.

flipPitchDirection

A Boolean specifying whether to override the direction of translation. If *flipPitchDirection*=OFF, the direction of translation is given by the direction of the revolve axis. If *flipPitchDirection*=ON, the translation direction is reversed. The default value is OFF.

moveSketchNormalToPath

A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath*=OFF, the sketch plane remains parallel to the revolve axis. If *moveSketchNormalToPath*=ON, the sketch is moved to match the angle created by the *pitch before being revolved. The default value is OFF.

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

ShellSweep(path: str, profile: str, pathPlane: str = '', pathUpEdge: ~abaqus.BasicGeometry.Edge.Edge = <abaqus.BasicGeometry.Edge.Edge object>, pathOrientation: ~abaqusConstants.SymbolicConstantType | None = None, sketchPlane: str = '', sketchUpEdge: ~abaqus.BasicGeometry.Edge.Edge = <abaqus.BasicGeometry.Edge.Edge object>, sketchOrientation: ~abaqusConstants.SymbolicConstantType | None = None, draftAngle: float | None = None, pitch: float | None = None, profileNormal: ~abaqusConstants.BooleanType = 0, flipSweepDirection: ~abaqusConstants.BooleanType = 0, keepInternalBoundaries: ~abaqusConstants.BooleanType = 0)

This method creates an additional Feature object by sweeping the given ConstrainedSketch object or a sequence of Edge objects along a path which may be a ConstrainedSketch or a sequence of Edge objects, creating a shell swept protrusion. The section can be an open or a closed profile. The section sketch can be created at the normal plane at the start of the sweep path or it may be created on a Datum plane or a planar Face. No checks are made for self-intersection.

Parameters:

path

Path may either be a ConstrainedSketch object or a sequence of Edge objects specifying the path of the sweep.

profile

Profile may either be a ConstrainedSketch object or a sequence of Edge objects specifying the section to be swept.

pathPlane

A Datum plane object or a planar Face object. Only required when path is a ConstrainedSketch object.

pathUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the path sketch. Only required when path is a ConstrainedSketch object.

pathOrientation

A SymbolicConstant specifying the orientation of pathUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when path is a ConstrainedSketch object.

sketchPlane

A Datum plane object or a planar Face object specifying the plane on which to sketch the profile. Not required when profile is a Face object. When profile is chosen as ConstrainedSketch object, user may or may not give this as input. If user does not give this as input, the normal plane at the start of the path will be the sketchPlane.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the profile sketch. Only required when profile is a ConstrainedSketch object.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when profile is a ConstrainedSketch object.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

profileNormal

A Boolean specifying whether to keep the profile normal same as original or varying through out the sweep path. When *profileNormal*=OFF, the profile normal will vary through out the sweep path. When *profileNormal*=ON, the profile normal will be same as original through out the sweep path. The default value is OFF.

flipSweepDirection

A Boolean specifying whether to flip the direction in which sweep operation will be performed. When *flipSweepDirection*=OFF, sweep operation will be performed in the direction of path direction. When *flipSweepDirection*=ON, sweep operation will be performed in the direction opposite to the path direction. The default value is OFF.

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Skin(name: str, faces: tuple[Face] = (), edges: tuple[Edge] = (), elementFaces: tuple[MeshFace] = (), elementEdges: tuple[MeshEdge] = ()) → Skin

This method creates a skin from a sequence of objects in a model database. At least one of the optional arguments needs to be specified.

Parameters:

name

A String specifying the repository key. The default value is an empty string.

faces

A sequence of Face objects specifying the faces on which skins should be created. Applicable to three and two-dimensional parts.

edges

A sequence of Edge objects specifying the edges on which skins should be created. Applicable to axisymmetric parts.

elementFaces

A sequence of MeshFace objects specifying the mesh faces on which skins should be created. Applicable to three and two-dimensional parts.

elementEdges

A sequence of MeshEdge objects specifying the mesh edges on which skins should be created. Applicable to axisymmetric parts.

Returns:

skin: Skin

A Skin object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].Skin

SolidExtrude(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, depth: float | None = None, upToFace: str = '', sketchOrientation: SymbolicConstantType = 'RIGHT', draftAngle: float | None = None, pitch: float | None = None, flipExtrudeDirection: BooleanType = 0, keepInternalBoundaries: BooleanType = 0)

This method creates an additional Feature object by extruding the given ConstrainedSketch object by the given depth, creating a solid protrusion. The ConstrainedSketch object must define a closed profile.

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketch

A ConstrainedSketch object specifying the planar sketch to be extruded.

depth

A Float specifying the extrusion depth. The default is to not specify a depth. Either depth or upToFace must be used to define the extrusion depth.

upToFace

A Face specifying the face up to which to extrude. If upToFace is specified, the extrusion will be an up-to-face extrusion. The default is to not specify a face. Either depth or upToFace must be used to define the extrusion depth.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

flipExtrudeDirection

A Boolean specifying whether to override the direction of feature creation. If the value is OFF, it means use the direction defined by the sketchPlaneSide; if the value is ON, it means use the opposite direction to the one defined by sketchPlaneSide. The default value is OFF.

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

SolidLoft(loftsections: tuple, startCondition: SymbolicConstantType | None = None, endCondition: SymbolicConstantType | None = None, startTangent: float | None = None, startMagnitude: float | None = None, endTangent: float | None = None, endMagnitude: float | None = None, paths: tuple = (), globalSmoothing: BooleanType = 0, keepInternalBoundaries: BooleanType = 0)

This method creates an additional Feature object by lofting between the given sections and adding material to the part. You define the sections using a sequence of edges from the part or an EdgeArray.

Parameters:

loftsections

A sequence of sequences of edges specifying the cross-sections to be lofted. Each outer sequence specifies a section through which Abaqus will pass the loft feature. Each outer sequence can be defined as a sequence of edges or as an EdgeArray. The edges specifying a section must form a simple closed profile and must not contain multiple loops.

startCondition

A SymbolicConstant specifying the tangent direction at the start section of the loft feature. Possible values are NONE, NORMAL, RADIAL and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the startCondition argument in conjunction with the endCondition argument.

endCondition

A SymbolicConstant specifying the tangent direction at the end section of the loft feature. Possible values are NONE, NORMAL, RADIAL and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the endCondition argument in conjunction with the startCondition argument.

startTangent

A Float specifying the angle in degrees of the tangent with respect to the plane in which the start section lies. You must specify the startTangent argument if startCondition*=SPECIFIED. Possible values are 0.0 ≤≤ *startTangent ≤≤ 180.0.

startMagnitude

A Float specifying the magnitude of the startTangent. You must specify the startMagnitude argument if startCondition*=SPECIFIED. Possible values are 0.0 << *startMagnitude << 100.0.

endTangent

A Float specifying the angle in degrees of the tangent with respect to the plane in which the end section lies. You must specify the endTangent argument if startCondition*=SPECIFIED. Possible values are 0.0 ≤≤ *endTangent ≤≤ 180.0.

endMagnitude

A Float specifying the magnitude of the endTangent. This argument is to be used when the endCondition argument has the value SPECIFIED. Possible values are 0.0 << endMagnitude << 100.0.

paths

A sequence of sequences of edges that pass through each section in the loft feature. Each sequence specifies a path followed by the face or an edge created by a loft feature. Each path must start at the first section, end at the last section, and pass through each section. In addition, the order of the sequences must be the same as the order of the sections in the loftsections argument. Each path must not self-intersect and must be tangent continuous. In addition, the paths must not intersect each other. You cannot use the paths argument in conjunction with the startCondition and endCondition arguments.

globalSmoothing

A Boolean specifying whether each path defined in the paths argument is applied locally or globally.If the path is applied locally, its effect is felt only on faces created from the edges on the loftsections through which the paths pass through.If the path is applied globally, an averaging algorithm is applied over all the paths defined and is distributed over all the faces created.The default value is ON (globally).

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

SolidRevolve(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, angle: float, sketchOrientation: SymbolicConstantType = 'RIGHT', pitch: float | None = None, flipRevolveDirection: BooleanType = 0, flipPitchDirection: BooleanType = 0, moveSketchNormalToPath: BooleanType = 0, keepInternalBoundaries: BooleanType = 0)

This method creates an additional Feature object by revolving the given ConstrainedSketch object by the given angle, creating a solid protrusion. The ConstrainedSketch object must define a closed profile and an axis of revolution. The axis is defined by a single construction line.

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketch

A ConstrainedSketch object specifying the planar sketch to be revolved.

angle

A Float specifying the angle in degrees to be revolved.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤≤ pitch ≤≤ 105. The default value, 0, implies a normal revolve.

flipRevolveDirection

A Boolean specifying whether to override the direction of feature creation. If *flipRevolveDirection*=OFF, the default direction of revolution is used. If *flipRevolveDirection*=ON, the revolve direction is reversed. The default value is OFF.

flipPitchDirection

A Boolean specifying whether to override the direction of translation. If *flipPitchDirection*=OFF, the direction of translation is given by the direction of the revolve axis. If *flipPitchDirection*=ON, the translation direction is reversed. The default value is OFF.

moveSketchNormalToPath

A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath*=OFF, the sketch plane remains parallel to the revolve axis. If *moveSketchNormalToPath*=ON, the sketch is moved to match the angle created by the *pitch before being revolved. The default value is OFF.

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

SolidSweep(path: str, profile: str, pathPlane: str = '', pathUpEdge: ~abaqus.BasicGeometry.Edge.Edge = <abaqus.BasicGeometry.Edge.Edge object>, pathOrientation: ~abaqusConstants.SymbolicConstantType | None = None, sketchPlane: str = '', sketchUpEdge: ~abaqus.BasicGeometry.Edge.Edge = <abaqus.BasicGeometry.Edge.Edge object>, sketchOrientation: ~abaqusConstants.SymbolicConstantType | None = None, draftAngle: float | None = None, pitch: float | None = None, profileNormal: ~abaqusConstants.BooleanType = 0, flipSweepDirection: ~abaqusConstants.BooleanType = 0, keepInternalBoundaries: ~abaqusConstants.BooleanType = 0)

This method creates an additional Feature object by sweeping the given ConstrainedSketch object or a Face object along a path which may be a ConstrainedSketch or a sequence of Edge objects, creating a solid swept protrusion. If the profile section is a ConstrainedSketch object, it must define a closed profile. The section sketch can be created at the normal plane at the start of the sweep path or it may be created on a Datum plane or a planar Face. No checks are made for self-intersection.

Parameters:

path

Path may either be a ConstrainedSketch object or a sequence of Edge objects specifying the path of the sweep.

profile

Profile may either be a ConstrainedSketch object or a Face object specifying the section to be swept.

pathPlane

A Datum plane object or a planar Face object. Only required when path is a ConstrainedSketch object.

pathUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the path sketch. Only required when path is a ConstrainedSketch object.

pathOrientation

A SymbolicConstant specifying the orientation of pathUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when path is a ConstrainedSketch object.

sketchPlane

A Datum plane object or a planar Face object specifying the plane on which to sketch the profile. Not required when profile is a Face object. When profile is chosen as ConstrainedSketch object, user may or may not give this as input. If user does not give this as input, the normal plane at the start of the path will be the sketchPlane.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the profile sketch. Only required when profile is a ConstrainedSketch object.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when profile is a ConstrainedSketch object.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

profileNormal

A Boolean specifying whether to keep the profile normal same as original or varying through out the sweep path. When *profileNormal*=OFF, the profile normal will vary through out the sweep path. When *profileNormal*=ON, the profile normal will be same as original through out the sweep path. The default value is OFF.

flipSweepDirection

A Boolean specifying whether to flip the direction in which sweep operation will be performed. When *flipSweepDirection*=OFF, sweep operation will be performed in the direction of path direction. When *flipSweepDirection*=ON, sweep operation will be performed in the direction opposite to the path direction. The default value is OFF.

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Stitch(edgeList: tuple[Edge] = (), stitchTolerance: float | None = None)

This method attempts to create a valid part by binding together free and imprecise edges of all the faces of a part. If edgeList is not given, a global stitch will be performed. If stitchTolerance is not specified, a value of 1.0 will be used.

Parameters:

edgeList

A sequence of Edge objects specifying the edges that need to be stitched.

stitchTolerance

A Float indicating the maximum gap to be stitched. The value should be smaller than the minimum feature size and bigger than the maximum gap expected to be stitched in the model. Otherwise this command may remove small (sliver) edges that are smaller than the tolerance.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Stringer(name: str, edges: tuple[Edge] = (), elementEdges: tuple[MeshEdge] = ()) → Stringer

This method creates a stringer from a sequence of objects in a model database. At least one of the optional arguments needs to be specified.

Parameters:

name

A String specifying the repository key. The default value is an empty string.

edges

A sequence of Edge objects specifying the edges on which stringers should be created. Applicable to three and two-dimensional parts.

elementEdges

A sequence of MeshEdge objects specifying the mesh edges on which stringers should be created. Applicable to three and two-dimensional parts.

Returns:

stringer: Stringer

A Stringer object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].Stringer

Surface(side1Faces: tuple[Face] | None = None, side2Faces: tuple[Face] | None = None, side12Faces: tuple[Face] | None = None, end1Edges: tuple[Face] | None = None, end2Edges: tuple[Face] | None = None, circumEdges: tuple[Face] | None = None, side1Edges: tuple[Face] | None = None, side2Edges: tuple[Face] | None = None, face1Elements: tuple[Face] | None = None, face2Elements: tuple[Face] | None = None, face3Elements: tuple[Face] | None = None, face4Elements: tuple[Face] | None = None, face5Elements: tuple[Face] | None = None, face6Elements: tuple[Face] | None = None, side1Elements: tuple[Face] | None = None, side2Elements: tuple[Face] | None = None, side12Elements: tuple[Face] | None = None, end1Elements: tuple[Face] | None = None, end2Elements: tuple[Face] | None = None, circumElements: tuple[Face] | None = None, name: str = '', **kwargs) → Surface

This method creates a surface from a sequence of objects in a model database. The surface will apply to the sides specified by the arguments.For example

surface=mdb.models['Model-1'].parts['Part-1'].Surface(side1Faces=side1Faces, name='Surf-1')

Parameters:

side1Faces

side2Faces

side12Faces

end1Edges

end2Edges

circumEdges

side1Edges

side2Edges

face1Elements

face2Elements

face3Elements

face4Elements

face5Elements

face6Elements

side1Elements

side2Elements

side12Elements

end1Elements

end2Elements

circumElements

name

A String specifying the repository key. The default value is an empty string.

Returns:

surf: Surface

A Surface object

Required key-value arguments

On three-dimensional solid faces, you can use the following arguments:

• side1Faces

• side2Faces

On three-dimensional shell faces, you can use the following arguments:

• side1Faces

• side2Faces

• side12Faces

On three-dimensional wire edges, you can use the following arguments:

• end1Edges

• end2Edges

• circumEdges

On three-dimensional or two-dimensional or axisymmetric edges, you can use the following arguments:

• side1Edges

• side2Edges

On two-dimensional or axisymmetric shell elements, you can use the following arguments:

• face1Elements

• face2Elements

• face3Elements

• face4Elements

On solid elements, you can use the following arguments:

• face1Elements

• face2Elements

• face3Elements

• face4Elements

• face5Elements

• face6Elements

On three-dimensional shell elements, you can use the following arguments:

• side1Elements

• side2Elements

• side12Elements

On three-dimensional wire elements, you can use the following arguments:

• end1Elements

• end2Elements

• circumElements

On two-dimensional or axisymmetric wire elements, you can use the following arguments:

• side1Elements

• side2Elements

Unlock()

This method unlocks the part. Unlocking the part allows it to be regenerated after any modifications to the part.

Wire(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, sketchOrientation: SymbolicConstantType = 'RIGHT')

This method creates an additional Feature object by creating a planar wire from the given ConstrainedSketch object. The ConstrainedSketch object must define a closed profile.

Parameters:

sketchPlane

A Datum plane object or a planar Face object specifying the plane on which to sketch.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketch

A ConstrainedSketch object specifying the planar sketch to be revolved.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

WireFromEdge(edgeList: str)

This method creates an additional Feature object by creating a Wire by selecting one or more Edge objects of a Solid or Shell part.

Parameters:

edgeList

A list of Edge objects specifying the edges from which the wire is to be created.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

WirePolyLine(points: tuple, mergeType: SymbolicConstantType = 'IMPRINT', meshable: BooleanType = 1)

This method creates an additional Feature object by creating a polyline wire that passes through a sequence of given points. Each point can be a datum point, a vertex, an interesting point, or a tuple.

Parameters:

points

A sequence of ConstrainedSketchVertex, Datum point, or InterestingPoint objects specifying the points through which the polyline wire will pass. points can also be a sequence of tuples of Floats. You must specify at least two values in the sequence.

mergeType

A SymbolicConstant specifying the merge behavior of the wire with existing geometry. If mergeType is MERGE, Abaqus merges the wire into solid regions of the part if the wire passes through them. If mergeType is IMPRINT, Abaqus imprints the wire on existing geometry as edges. If mergeType is SEPARATE, Abaqus neither merges nor imprints the spline wire with existing geometry. It creates the wire separately. The default value is IMPRINT.

meshable

A Boolean specifying whether the wire should be available for selection in meshing operations. If *meshable*=OFF, the wire can be used for connector section assignment. The default value is ON.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

WireSpline(points: tuple, mergeType: SymbolicConstantType = 'IMPRINT', smoothClosedSpline: BooleanType = 0)

This method creates an additional Feature object by creating a spline wire that passes through a sequence of given points. Each point can be a datum point, a vertex, an interesting point, or a tuple.

Parameters:

points

A sequence of ConstrainedSketchVertex, Datum point, or InterestingPoint objects specifying the points through which the spline wire will pass. points can also be a sequence of tuples of Floats. You must specify at least two values in the sequence.

mergeType

A SymbolicConstant specifying the merge behavior of the wire with existing geometry. If mergeType is MERGE, Abaqus merges the wire into solid regions of the part if the wire passes through them. If mergeType is IMPRINT, Abaqus imprints the spline wire on existing geometry as edges. If mergeType is SEPARATE, Abaqus neither merges nor imprints the spline wire with existing geometry. It creates the wire separately. The default value is IMPRINT.

smoothClosedSpline

A Boolean specifying the behavior of Abaqus when the points defining a spline wire form a closed loop (the start and end points are the same). If *smoothClosedSpline*=ON, Abaqus creates a smooth spline wire where the tangencies at the end point meet smoothly. If *smoothClosedSpline*=OFF, Abaqus does not automatically create a smooth end condition. The default value in OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

addGeomToSketch(sketch: ConstrainedSketch)

This method converts a part into a sketch by projecting all of the edges of the part onto the X-Y plane of the sketch. You can use addGeomToSketch with a part of any modeling space.

Parameters:

sketch

A ConstrainedSketch object.

adjustMidsideNode(cornerNodes: tuple[abaqus.EditMesh.MeshEditPart.Node], parameter: float)

This method is used to adjust the midside node of second-order elements of an orphan mesh part.

Parameters:

cornerNodes

A sequence of Node objects specifying the nodes towards which connected midside nodes will be biased.

parameter

A Float specifying the normalized distance along the edge of the midside nodes. Possible values are 0.0 ≤≤ parameter ≤≤ 1.0, where 0.0 specifies the position of the corner node. The default value is 0.5.

assignStackDirection(cells: tuple[Cell], referenceRegion: Face)

This method assigns a stack direction to geometric cells. The stack direction will be used to orient the elements during mesh generation.

Parameters:

cells

A sequence of Cell objects specifying regions where to assign the stack direction.

referenceRegion

A Face object specifying the top side of the stack direction.

assignThickness(faces: tuple[Face], thickness: float | None = None, topFaces: tuple[Face] = (), bottomFaces: tuple[Face] = ())

This method assigns thickness data to shell faces. The thickness can be used while assigning shell and membrane sections to faces.

Parameters:

faces

A sequence of Face objects specifying the regions where thickness will be applied.

thickness

A Float specifying the thickness along the given faces . Either thickness, topFaces, or bottomFaces must be specified.

topFaces

A sequence of Face objects whose distance to faces argument is used to calculate the thickness along the faces. The combination of topFaces and bottomFaces determines the thickness and the offset of the elements. If bottomFaces is not specified then the thickness is twice the distance to the topFaces. This argument will be ignored if thickness is specified. Either thickness, topFaces, or bottomFaces must be specified.

bottomFaces

A sequence of Face objects whose distance to faces is used to calculate the thickness along the faces. The combination of topFaces and bottomFaces determines the thickness and the offset of the elements. If topFaces is not specified then the thickness is twice the distance to the bottomFaces. This argument will be ignored if thickness is specified. Either thickness, topFaces, or bottomFaces must be specified.

associateMeshWithGeometry(geometricEntity: str, elements: tuple[abaqus.Mesh.MeshElement.MeshElement] = (), elemFaces: tuple[abaqus.Mesh.MeshFace.MeshFace] = (), elemEdges: tuple[abaqus.Mesh.MeshEdge.MeshEdge] = (), node: ~abaqus.Mesh.MeshNode.MeshNode = <abaqus.Mesh.MeshNode.MeshNode object>)

This method associates a geometric entity with mesh entities that are either orphan elements, bounds orphan elements, or were created using the bottom-up meshing technique.

Parameters:

geometricEntity

A Cell, a Face, an Edge, or a ConstrainedSketchVertex object specifying geometric entity to be associated with one or more mesh entities.If the geometric entity is a Cell object then the argument elements must be specified.If the geometric entity is a Face object then the argument elemFaces must be specified.If the geometric entity is an Edge object then the argument elemEdges must be specified.If the geometric entity is a ConstrainedSketchVertex object then the argument node must be specified.

elements

A sequence of MeshElement objects specifying the elements to be associated with the geometric cell.

elemFaces

A sequence of MeshFace objects specifying the element faces to be associated with the geometric face.

elemEdges

A sequence of MeshEdge objects specifying the element edges to be associated with the geometric edge.

node

A MeshNode object specifying the mesh node to be associated with the geometric vertex.

backup()

This method makes a backup copy of the features in the part. Use the restore method to retrieve the part’s features from the backup.

checkGeometry(detailed: BooleanType = 0, reportFacetErrors: BooleanType = 0, level: int | None = None)

This method checks the validity of the geometry of the part and prints a count of all topological entities on the part (faces, edges, vertices, etc.).

Parameters:

detailed

A Boolean specifying whether detailed output will be printed to the replay file. The default value is OFF.

reportFacetErrors

A Boolean specifying whether faces are checked for proper facetting. The default value is OFF.

level

An Int specifying which level of checking is performed. Values can range from 20 to 70, with higher values reporting less and less important errors. The default value is 20, which reports all critical errors. When the default value is used, the stored validity status is updated to agree with the result of this check.

clashSets(arg1: str, arg2: str)

This command prints a message describing the relationship between the contents of two sets. Possible outcomes are:

• Both sets are the same.

• Set 2 is a subset of set 1.

• Set 2 is a superset of set 1.

• Set 2 intersects set 1.

• Set 2 touches set 1 (their boundaries intersect).

• Set 2 and set 1 are disjoint.

This command accepts only positional arguments and has no keywords.

Parameters:

arg1

A Set or Surface object specifying set 1.

arg2

A Set or Surface object specifying set 2.

cleanMesh(mergeTolerance: float, growEdges: BooleanType = 0, elements: str = '', refEdge: str = '', thicknessDir: float | None = None, moveLayers: BooleanType = False)

This method is used to collapse short element edges and delete collapsed elements, or grow short element edges, on an orphan mesh part composed of linear elements.

Parameters:

mergeTolerance

A Float specifying the edge length tolerance. During the operation, edges shorter than the given tolerance will be collapsed, or grown to the specified length.

growEdges

A Boolean specifying whether short element edges will be grown to the specified tolerance. Default is False, meaning short edges will be collapsed.

elements

The elements to consider as the domain for the operation. By default all elements on the part are considered. The elements may be given as a MeshElementArray, a list of MeshElement objects, a Set, or a list of Set objects.

refEdge

A MeshEdge specifying a reference edge to indicate a topological direction in a structured mesh that will limit which edges within the element domain are considered. That is, only edges that are found to be topologically parallel to the given reference edge will be considered by the operation. By default all edges of the element domain are considered, unless thicknessDir is specified, in which case the operation will attempt to determine the topological edges from the thickness direction.

thicknessDir

A tuple of two or three Floats indicating a vector along which element edge lengths will be measured.

moveLayers

A Boolean indicating whether element edges will be all grown in the direction of the thickness vector specified by thicknessDir. This argument is ignored unless growEdges is True and thicknessDir is provided. When this argument is True the growth of any given element edge will no longer be constrained by short edges on neighboring elements, but elements could move from their original positions in cases where there are multiple adjacent layers of thin elements. The default value is False.

clearGeometryCache()

This method clears the geometry cache. Clearing the geometry cache reduces the amount of memory being used to cache part features.

collapseMeshEdge(edge: str, collapseMethod: SymbolicConstantType)

This method collapses an edge of a quadrilateral or triangular element of an orphan mesh part or part instance.

Parameters:

edge

A single MeshEdge object specifying the element edge to collapse.

collapseMethod

A SymbolicConstant specifying the method used to collapse the edge. Possible values are FORWARD, REVERSE, and AVERAGE.

combineElement(elements: tuple)

This method combines two triangular elements of an orphan mesh part or an Abaqus native mesh.

Parameters:

elements

A sequence of triangular MeshElement objects specifying the elements to combine.

convertSolidMeshToShell()

This method removes all solid elements from an orphan mesh part and creates triangular or quadrilateral shell elements along their outer faces.

copyMeshPattern(elements: tuple[abaqus.Mesh.MeshElement.MeshElement] = (), faces: tuple[abaqus.BasicGeometry.Face.Face] = (), elemFaces: tuple[abaqus.Mesh.MeshFace.MeshFace] = (), targetFace: ~abaqus.Mesh.MeshFace.MeshFace = <abaqus.Mesh.MeshFace.MeshFace object>, nodes: tuple[abaqus.Mesh.MeshNode.MeshNode] = (), coordinates: tuple = ())

This method copies a mesh pattern from a source region consisting of a set of shell elements or element faces onto a target face, mapping nodes and elements in a one-one correspondence between source and target.

Parameters:

elements

A sequence of MeshElement objects or a Set object containing elements and specifying the source region.

faces

A sequence of Face objects that have associated with shell elements or element faces and specifying the source region.

elemFaces

A sequence of MeshFace objects specifying the source region.

targetFace

A MeshFace object specifying the target region.

nodes

A sequence of MeshNode objects or a Set object containing nodes on the boundary of source region which are to be positioned to the boundary of target face.

coordinates

A sequence of three-dimensional coordinate tuples specifying the coordinates for each of the given nodes. When specified, the number of coordinate tuples must match the number of given nodes, and be ordered to correspond to the given nodes in ascending order according to index. These coordinates are positions of the nodes of a mesh that will be the target face corresponding to nodes provided.

createVirtualTopology(regions: tuple[Face] = (), mergeShortEdges: BooleanType = False, shortEdgeThreshold: float | None = None, mergeSmallFaces: BooleanType = False, smallFaceAreaThreshold: float | None = None, mergeSliverFaces: BooleanType = False, faceAspectRatioThreshold: float | None = None, mergeSmallAngleFaces: BooleanType = False, smallFaceCornerAngleThreshold: float | None = None, mergeThinStairFaces: BooleanType = False, thinStairFaceThreshold: float | None = None, ignoreRedundantEntities: BooleanType = False, cornerAngleTolerance: float = 30, applyBlendControls: BooleanType = False, blendSubtendedAngleTolerance: float | None = None, blendRadiusTolerance: float | None = None)

This method creates a virtual topology feature by automatically merging faces and edges based on a set of geometric parameters. The edges and vertices that are being merged will be ignored during mesh generation.

Parameters:

regions

A sequence of Face objects specifying the domain to search for geometric entities that need to be merged. Entities identified as candidates to be merged may be merged with entities from outside the specified region. If regions is not specified then the entire part is the domain for searching geometric entities that need to be merged.

mergeShortEdges

A Boolean specifying whether to merge short edges. The default value is False.

shortEdgeThreshold

A Float specifying a threshold that determines which edges are considered to be short. These edges are the candidate entities to be merged. This argument is a required argument if the argument*mergeShortEdges* equals True and it is ignored if the argument mergeShortEdges equals False.

mergeSmallFaces

A Boolean specifying whether to merge faces with small area. The default value is False.

smallFaceAreaThreshold

A Float specifying a threshold that determines which faces are considered to have a small area. These faces are the candidate entities to be merged. This argument is a required argument if the argument*mergeSmallFaces* equals True and it is ignored if the argument mergeSmallFaces equals False.

mergeSliverFaces

A Boolean specifying whether to merge faces with high aspect ratio. The default value is False.

faceAspectRatioThreshold

A Float specifying a threshold that determines which faces are considered to have high aspect ratio. These faces are the candidate entities to be merged. This argument is a required argument if the argument*mergeSliverFaces* equals True and it is ignored if the argument mergeSliverFaces equals False.

mergeSmallAngleFaces

A Boolean specifying whether to merge faces that have a sharp corner angle. The default value is False.

smallFaceCornerAngleThreshold

A Float specifying a threshold that determines which face corner angles are considered to be small. These faces will be candidate entities to be merged. This argument is a required argument if the argument*mergeSmallAngleFaces* equals True and it is ignored if the argument mergeSmallAngleFaces equals False.

mergeThinStairFaces

A Boolean specifying whether to merge faces that represent a thin stair-like feature. The default value is False.

thinStairFaceThreshold

A Float specifying a threshold that determines which faces representing small stair-like features are considered thin. These faces will be candidate entities to be merged. This argument is required if the argument mergeThinStairFaces is True and it is ignored if mergeThinStairFaces is False.

ignoreRedundantEntities

A Boolean specifying whether to abstract away redundant edges and vertices. The default value is False.

cornerAngleTolerance

A Float specifying the angle deviation from 180 degrees at a vertex or at an edge such that the two edges radiating from the vertex or the two faces bounded by the edge can be merged. The default value is 30.0 degrees.

applyBlendControls

A Boolean specifying whether to verify that blend faces can be merged with neighboring faces. If applyBlendControls is true then all faces that have angle larger than blendSubtendedAngleTolerance and a radius smaller than blendRadiusTolerance will not be merged with neighboring faces unless the neighboring faces are also blend faces with similar geometric characteristics. The default value is False.

blendSubtendedAngleTolerance

A Float specifying the largest subtended angle of blend faces that can be merged with neighboring faces. This argument is a required argument if the argument applyBlendControls equals True and it is ignored if the argument applyBlendControls equals False.

blendRadiusTolerance

A Float specifying the smallest radius of curvature of blend faces that can be merged with neighboring faces. This argument is a required argument if the argument applyBlendControls equals True and it is ignored if the argument applyBlendControls equals False.

Returns:

feature: Feature

A Feature object

deleteAllFeatures()

This method deletes all the features in the part.

deleteBoundaryLayerControls(regions: tuple[Cell])

This method deletes the control parameters for boundary layer mesh for all the specified regions.

Parameters:

regions

A sequence of Cell objects specifying the regions for which to set the boundary layer mesh control parameters.

deleteElement(elements: tuple[MeshElement], deleteUnreferencedNodes: BooleanType = 0)

This method deletes the given elements from an orphan mesh part or an Abaqus native mesh. If the elements belong to an Abaqus native mesh then the elements must have been generated using the bottom-up meshing technique.

Parameters:

elements

A sequence of MeshElement objects or a Set object containing elements.

deleteUnreferencedNodes

A Boolean specifying whether to delete all those associated nodes that become unreferenced after the given elements are deleted. The default value is OFF.

deleteFeatures(featureNames: tuple)

This method deletes the given features.

Parameters:

featureNames

A sequence of Strings specifying the feature names that will be deleted from the part.

deleteMesh(regions: tuple['Part'])

This method deletes a subset of the mesh that contains the native elements from the given parts or regions.

Parameters:

regions

A sequence of Part objects or Region objects specifying the parts or regions from which the native mesh is to be deleted.

deleteMeshAssociationWithGeometry(geometricEntities: tuple[Cell], addBoundingEntities: BooleanType = False)

This method deletes the association of geometric entities with mesh entities.

Parameters:

geometricEntities

A sequence of Cell objects, Face objects, Edge objects, or ConstrainedSketchVertex objects specifying the geometric entities that will be disassociated from the mesh.

addBoundingEntities

A Boolean specifying whether the mesh will also be disassociated from the geometric entities that bounds the given geometricEntities. For example, if the argument geometricEntities contains a face, this boolean indicates whether the edges and vertices that bound the face will also be disassociated from the mesh. The default value is False.

deleteNode(nodes: tuple[MeshNode], deleteUnreferencedNodes: BooleanType = 0)

This method deletes the given nodes from an orphan mesh part.

Parameters:

nodes

A sequence of MeshNode objects or a Set object containing nodes.

deleteUnreferencedNodes

A Boolean specifying whether to delete all those associated nodes that become unreferenced after the given nodes and the connected elements are deleted. The default value is OFF.

deletePreviewMesh()

This method deletes all boundary meshes in the parts. See the boundaryPreview argument of generateMesh for information about generating boundary meshes.

deleteSeeds(regions: tuple['Part'])

This method deletes the global edge seeds from the given parts or deletes the local edge seeds from the given edges.

Parameters:

regions

A sequence of Part objects or Edge objects specifying the parts or edges from which the seeds are to be deleted.

deleteSets(setNames: tuple)

This command deletes the given sets from the part.

Parameters:

setNames

A sequence of Strings specifying the set names that will be deleted from the part.

deleteSurfaces(surfaceNames: tuple)

This command deletes the given surfaces from the part.

Parameters:

surfaceNames

A sequence of Strings specifying the surface names that will be deleted from the part.

editNode(nodes: tuple[abaqus.Mesh.MeshNode.MeshNode], coordinate1: float | None = None, coordinate2: float | None = None, coordinate3: float | None = None, coordinates: tuple = (), offset1: float | None = None, offset2: float | None = None, offset3: float | None = None, localCsys: ~abaqus.Datum.DatumCsys.DatumCsys = <abaqus.Datum.DatumCsys.DatumCsys object>, projectToGeometry: ~abaqusConstants.BooleanType = 1)

This method changes the coordinates of the given nodes on an orphan mesh part or on an Abaqus native mesh.

Parameters:

nodes

A sequence of MeshNode objects or a Set object containing nodes.

coordinate1

A Float specifying the value of the first coordinate. If coordinate1 and offset1 are unspecified, the existing value does not change.

coordinate2

A Float specifying the value of the second coordinate. If coordinate2 and offset2 are unspecified, the existing value does not change.

coordinate3

A Float specifying the value of the third coordinate. If coordinate3 and offset3 are unspecified, the existing value does not change.

coordinates

A sequence of three-dimensional coordinate tuples specifying the coordinates for each of the given nodes. When specified, the number of coordinate tuples must match the number of given nodes, and be ordered to correspond to the given nodes in ascending order according to index. Furthermore, coordinate1, coordinate2, coordinate3, offset1, offset2, or offset3 may not be specified.

offset1

A Float specifying an offset to apply to the value of the first coordinate of the specified nodes.

offset2

A Float specifying an offset to apply to the value of the second coordinate of the specified nodes.

offset3

A Float specifying an offset to apply to the value of the third coordinate of the specified nodes.

localCsys

A DatumCsys object specifying the local coordinate system. If unspecified, the global coordinate system will be used.

projectToGeometry

A Boolean specifying whether to project nodes back to their original geometry. For example, if a node is on a face, this method first positions the node at the new location and then projects it back to the original face. The default value is ON.

Raises:

A coordinate and an offset may not both be specified for the same coordinate component.

generateBottomUpExtrudedMesh(cell: Cell, numberOfLayers: int, extrudeVector: tuple, geometrySourceSide: str = '', elemFacesSourceSide: tuple[MeshFace] = (), elemSourceSide: tuple = (), depth: float | None = None, targetSide: str = '', biasRatio: float = 1, extendElementSets: BooleanType = False)

This method generates solid elements by extruding a 2D mesh along a vector, either on an orphan mesh or within a cell region using a bottom-up technique.

Parameters:

cell

A Cell object specifying the geometric region where the mesh is to be generated. This argument is valid only for native parts.

numberOfLayers

An Int specifying the number of layers to be generated along the extrusion vector.

extrudeVector

A sequence of sequences of Floats specifying the start point and end point of a vector. Each point is defined by a tuple of three coordinates indicating its position. The direction of the mesh extrusion operation is from the first point to the second point.

geometrySourceSide

A Region of Face objects specifying the geometric domain to be used as the source for the extrude meshing operation.

elemFacesSourceSide

A sequence of MeshFace objects specifying the faces of 3D elements to be used as the source for the extrude meshing operation.

elemSourceSide

A sequence of 2D MeshElement objects specifying the elements to be used as the source for the extrude meshing operation.

depth

A Float specifying the distance of the mesh extrusion. If unspecified, the vector length of the extrudeVector argument is assumed.

targetSide

A datum plane, a sequence of Face objects, a sequence of MeshFace objects, or a sequence of 2D MeshElement objects specifying the target of the extrude meshing operation. If specified, this argument overrides the depth argument, and all points on the source will be extruded in the direction of the extrusion vector until meeting the target.

biasRatio

A Float specifying a ratio of the element size in the extrusion direction between the source and the target sides of the extrusion. The default is 1.0, meaning no bias.

extendElementSets

A Boolean specifying whether existing element sets that include source elements will be extended to also include extruded elements. This argument is ignored for native parts. The default value is False.

generateBottomUpRevolvedMesh(cell: Cell, numberOfLayers: int, axisOfRevolution: tuple, angleOfRevolution: float, geometrySourceSide: str = '', elemFacesSourceSide: tuple[MeshFace] = (), elemSourceSide: tuple = (), extendElementSets: BooleanType = False)

This method generates solid elements by revolving a 2D mesh around an axis, either on an orphan mesh or within a cell region using a bottom-up technique.

Parameters:

cell

A Cell object specifying the geometric region where the mesh is to be generated. This argument is valid only for native parts.

numberOfLayers

An Int specifying the number of layers of elements to be generated around the axis of revolution.

axisOfRevolution

A sequence of sequences of Floats specifying the two points of the vector that describes the axis of revolution. Each point is defined by a tuple of three coordinates indicating its position. The direction of the axis of revolution is from the first point to the second point. The orientation of the revolution operation follows the right-hand-rule about the axis of revolution.

angleOfRevolution

A Float specifying the angle of revolution.

geometrySourceSide

A Region of Face objects specifying the geometric domain to be used as the source for the revolve meshing operation.

elemFacesSourceSide

A sequence of MeshFace objects specifying the faces of 3D elements to be used as the source for the revolve meshing operation.

elemSourceSide

A sequence of 2D MeshElement objects specifying the elements to be used as the source for the revolve meshing operation.

extendElementSets

A Boolean specifying whether existing element sets that include source elements will be extended to also include extruded elements. This argument is ignored for native parts. The default value is False.

generateBottomUpSweptMesh(cell: ~abaqus.BasicGeometry.Cell.Cell, geometrySourceSide: str = '', elemFacesSourceSide: tuple[abaqus.Mesh.MeshFace.MeshFace] = (), elemSourceSide: tuple = (), geometryConnectingSides: str = '', elemFacesConnectingSides: tuple[abaqus.Mesh.MeshFace.MeshFace] = (), elemConnectingSides: tuple = (), targetSide: ~abaqus.BasicGeometry.Face.Face = <abaqus.BasicGeometry.Face.Face object>, numberOfLayers: int | None = None, extendElementSets: ~abaqusConstants.BooleanType = False)

This method generates solid elements by sweeping a 2D mesh, either on an orphan mesh or within a cell region using a bottom-up technique.

Parameters:

cell

A Cell object specifying the geometric region where the mesh is to be generated. This argument is valid only for native parts.

geometrySourceSide

A Region of Face objects specifying the geometric domain to be used as the source for the sweep meshing operation.

elemFacesSourceSide

A sequence of MeshFace objects specifying the faces of 3D elements to be used as the source for the sweep meshing operation.

elemSourceSide

A sequence of 2D MeshElement objects specifying the elements to be used as the source for the sweep meshing operation.

geometryConnectingSides

A Region of Face objects specifying connecting sides of the sweep meshing operation.

elemFacesConnectingSides

A sequence of MeshFace objects specifying connecting sides of the sweep meshing operation.

elemConnectingSides

A sequence of 2D MeshElement objects specifying connecting sides of the sweep meshing operation.

targetSide

A Face object specifying the target side of the sweep meshing operation.

numberOfLayers

An Int specifying the number of layers to be generated along the sweep direction.

extendElementSets

A Boolean specifying whether existing element sets that include source elements will be extended to also include swept elements. This argument is ignored for native parts. The default value is False.

generateMesh(elemShape: SymbolicConstantType | None = None)

This method generates a new mesh on an orphan mesh part based on the original mesh.

Parameters:

elemShape

A SymbolicConstant specifying the element shape to be used for meshing. Possible values are:TRIRefine a planar triangular mesh and replace it with a new one. If no element sizes are attached, the new mesh will be governed by the sizes of the boundary edges in the old mesh.TETCreate a tetrahedral mesh from a closed shell of triangular elements.

generateMeshByOffset(region: Region, meshType: str, totalThickness: float, distanceBetweenLayers: float, numLayers: int, offsetDirection: str = 'OUTWARD', initialOffset: float = 0.0, shareNodes: str = False, deleteBaseElements: BooleanType = False, constantThicknessCorners: BooleanType = False, extendElementSets: BooleanType = False)

This method generates a solid or shell mesh from an orphan mesh surface by generating layers of elements that propagate out normal to the surface boundary.

Parameters:

region

A Region object specifying the domain to be offset.

meshType

A Symbolic Constant specifying the type of mesh to be generated. Possible values are SOLID or SHELL.

totalThickness

A Float specifying the total thickness of the solid layers. This argument applies only when *meshType*=SOLID.

distanceBetweenLayers

A Float specifying the distance between shell layers. This argument applies only when *meshType*=SHELL.

numLayers

An Int specifying the number of element layers to be generated.

offsetDirection

A Symbolic Constant specifying the direction of the offset. This argument is required only when the given region relates to a shell mesh. Possible values are OUTWARD, INWARD, and BOTH. The default value is OUTWARD.

initialOffset

A Float specifying the magnitude of the initial offset. The default value is zero.

shareNodes

Boolean specifying whether the first layer of nodes should be shared with nodes on the base surface. The default value is False.

deleteBaseElements

A Boolean specifying whether to delete the shell elements after the offset layers are generated. The default value is False. This argument applies only when *meshType*=SHELL.

constantThicknessCorners

A Boolean specifying whether to use element-based thickness or nodal-based thickness. The default value is False.

extendElementSets

A Boolean specifying whether existing element sets that include base elements will be extended to include corresponding offset elements. The default value is False.

getAngle(plane1: str, plane2: str, line1: str, line2: str, commonVertex: str = '')

This method returns the angle between the specified entities.

Parameters:

plane1

A Face, MeshFace, or a Datum object specifying the first plane. The Datum object must represent a datum plane. The plane1 and line1 arguments are mutually exclusive. One of them must be specified.

plane2

A Face, MeshFace, or a Datum object specifying the second plane. The Datum object must represent a datum plane. The plane2 and line2 arguments are mutually exclusive. One of them must be specified.

line1

An Edge, MeshEdge, or a Datum object specifying the first curve. The Datum object must represent a datum axis. The plane1 and line1 arguments are mutually exclusive. One of them must be specified.

line2

An Edge, MeshEdge, or a Datum object specifying the second curve. The Datum object must represent a datum axis. The plane2 and line2 arguments are mutually exclusive. One of them must be specified.

commonVertex

If the two selected Edge objects have more than one vertex in common, this ConstrainedSketchVertex object specifies the vertex at which to evaluate the angle.

Returns:

angle: python:float

A Float specifying the angle between the specified entities. If you provide a plane as an argument, Abaqus/CAE computes the angle using the normal to the plane.

getArea(faces: tuple[Face], relativeAccuracy: float = 0)

This method returns the total surface area of a given face or group of faces.

Parameters:

faces

A sequence of Face objects whose area the method will calculate.

relativeAccuracy

A Float specifying that the area computation should stop when the specified relative accuracy has been achieved. The default value is 0.000001 (0.0001%).

Returns:

area: python:float

A Float specifying the sum of the calculated areas of the given faces.

getAssociatedCADPaths()

This method returns the paths to the associated CAD part and root file. These are only available if the part was imported from one of the supported CAD softwares using the Associative Import capability. The root file can be the assembly file or the part file, depending on what which one was imported.

Returns:

paths: python:tuple

A sequence containing the path to the associated CAD part and assembly file

getCADParameters()

This method returns the names and values of the CAD parameters associated with the part. These are only available if the part was imported from one of the supported CAD softwares using the Associative Import capability, and if the parameter names defined in that CAD software are prefixed with the string ABQ.

Returns:

paras: python:dict

A dictionary object representing a map of the name of the parameter and its associated value.

getCentroid(faces: tuple[Face], cells: tuple[Face], relativeAccuracy: float = 0)

Depending on the arguments provided, this method returns the following:

• The location of the centroid of a given face or group of faces.

• The location of the centroid of a given cell or group of cells.

faces

A sequence of Face objects whose centroid the method will calculate. The arguments faces and cells are mutually exclusive.

cells

A sequence of Face objects whose centroid the method will calculate. The arguments faces and cells are mutually exclusive.

relativeAccuracy

A Float specifying that the centroid computation should stop when the specified relative accuracy has been achieved. The default value is 0.000001 (0.0001%).

Returns:

centroid: python:tuple[python:float]

A sequence of Floats specifying the X-, Y-, and Z-coordinates of the centroid.

getCoordinates(entity: str, csys: DatumCsys)

This method returns the coordinates of specified point.

Parameters:

entity

A ConstrainedSketchVertex, Datum point, MeshNode, or ReferencePoint specifying the entity to query.

csys

A DatumCsys object specifying the desired coordinate system of the returned coordinates. By default, coordinates are given in the global coordinate system.

Returns:

A python:tuple of 3 Floats representing the coordinates of the specified point.

getCurvature(edges: tuple[Edge], samplePoints: int = 100)

This method returns the maximum curvature of a given edge or group of edges. For an arc, the curvature is constant over the entire edge, and equal to the inverse of the radius. For a straight line, the curvature is constant and equal to 0. For a spline edge, the curvature varies over a range, and this methods computes the maximum.

Parameters:

edges

A sequence of Edge objects whose curvature the method will calculate.

samplePoints

An Int specifying the number of points along each edge at which the curvature will be computed. The higher the number of sample points, the better the accuracy of the computation. The default value is 100.

Returns:

curvature: python:float

A Float specifying the maximum curvature.

getDistance(entity1: str, entity2: str)

Depending on the arguments provided, this method returns one of the following:

• The distance between two points.

• The minimum distance between a point and an edge.

• The minimum distance between two edges.

Parameters:

entity1

A ConstrainedSketchVertex, Datum point, MeshNode, or Edge specifying the first entity from which to measure.

entity2

A ConstrainedSketchVertex, Datum point, MeshNode, or Edge specifying the second entity to which to measure.

Returns:

distance: python:float

A Float specifying the distance between entity1 and entity2.

getEdgeSeeds(edge: Edge, attribute: SymbolicConstantType | float)

This method returns an edge seed parameter for a specified edge of a part.

Parameters:

edge

An Edge object specifying the edge to be queried.

attribute

A SymbolicConstant specifying the type of edge seed attribute to return. Possible values are:

• EDGE_SEEDING_METHOD

• BIAS_METHOD

• NUMBER

• AVERAGE_SIZE

• DEVIATION_FACTOR

• MIN_SIZE_FACTOR

• BIAS_RATIO

• BIAS_MIN_SIZE

• BIAS_MAX_SIZE

• VERTEX_ADJ_TO_SMALLEST_ELEM

• SMALLEST_ELEM_LOCATION

• CONSTRAINT

The return value is dependent on the attribute argument. - If *attribute*=EDGE_SEEDING_METHOD, the return value is a SymbolicConstant specifying the edge seeding method used to create the seeds along the edge. Possible values are:

• UNIFORM_BY_NUMBER

• UNIFORM_BY_SIZE

• CURVATURE_BASED_BY_SIZE

• BIASED

• NONE

• If *attribute*=BIAS_METHOD, the return value is a SymbolicConstant specifying the bias

type used to create the seeds along the edge. Possible values are:

• SINGLE

• DOUBLE

• NONE

• If *attribute*=NUMBER, the return value is an Int specifying the number of element

seeds along the edge. - If *attribute*=AVERAGE_SIZE, the return value is a Float specifying the average element size along the edge. - If *attribute*=DEVIATION_FACTOR, the return value is a Float specifying the deviation factor h/Lh/L, where hh is the chordal deviation and LL is the element length. If edge seeds are not defined, the return value is zero. - If *attribute*=MIN_SIZE_FACTOR, the return value is a Float specifying the size of the smallest allowable element as a fraction of the specified global element size. If edge seeds are not defined, the return value is zero. - If *attribute*=BIAS_RATIO, the return value is a Float specifying the length ratio of the largest element to the smallest element. - If *attribute*=BIAS_MIN_SIZE, the return value is a Float specifying the length of the largest element; only applicable if the EDGE_SEEDING_METHOD is BIASED and seeds were specified by minimum and maximum sizes. - If *attribute*=BIAS_MAX_SIZE, the return value is a Float specifying the length of the largest element; only applicable if the EDGE_SEEDING_METHOD is BIASED and seeds were specified by minimum and maximum sizes. - If *attribute*=VERTEX_ADJ_TO_SMALLEST_ELEM, the return value is an Int specifying the ID of the vertex next to the smallest element; only applicable if the EDGE_SEEDING_METHOD is BIASED. - If *attribute*=SMALLEST_ELEM_LOCATION, the return value is a SymbolicConstant specifying the location of smallest elements for double bias seeds; only applicable if the EDGE_SEEDING_METHOD is BIASED and BIAS_METHOD is DOUBLE. Possible values are:

• SMALLEST_ELEM_AT_CENTER

• SMALLEST_ELEM_AT_ENDS

• NONE

• If *attribute*=CONSTRAINT, the return value is a SymbolicConstant specifying how close

the seeds must be matched by the mesh. Possible values are:

• FREE

• FINER

• FIXED

• NONE

A value of NONE indicates that the edge is not seeded.

Returns:

The return value is a Float, an Int, or a SymbolicConstant depending on the value of the

attribute argument.

getElementType(region: str, elemShape: SymbolicConstantType)

This method returns the ElemType object of a given element shape assigned to a region of a part.

Parameters:

region

A Cell, a Face, or an Edge object specifying the region to be queried.

elemShape

A SymbolicConstant specifying the shape of the element for which to return the element type. Possible values are:

• LINE

• QUAD

• TRI

• HEX

• WEDGE

• TET

Returns:

ElemType object.

Raises:

• TypeError

  The region cannot be associated with element types or the elemShape is not

consistent with the dimension of the region.

getFeatureCells(name: str)

This method returns a sequence of Cell objects that are created by the given feature.

Parameters:

name

A string specifying the feature name.

Returns:

cells: python:tuple[Cell]

Sequence of Cell objects.

Raises:

• An exception occurs if a feature with the given name does not exist.

  Error : Incorrect feature name.

getFeatureEdges(name: str)

This method returns a sequence of Edge objects that are created by the given feature.

Parameters:

name

A string specifying the feature name.

Returns:

edges: python:tuple[Edge]

Sequence of Edge objects.

Raises:

• An exception occurs if a feature with the given name does not exist.

  Error : Incorrect feature name.

getFeatureFaces(name: str)

This method returns a sequence of Face objects that are created by the given feature.

Parameters:

name

A string specifying the feature name.

Returns:

faces: python:tuple[Face]

Sequence of Face objects.

Raises:

• An exception occurs if a feature with the given name does not exist.

  Error : Incorrect feature name.

getFeatureVertices(name: str)

This method returns a sequence of ConstrainedSketchVertex objects that are created by the given feature.

Parameters:

name

A string specifying the feature name.

Returns:

vertices: python:tuple[ConstrainedSketchVertex]

Sequence of ConstrainedSketchVertex objects.

Raises:

• An exception occurs if a feature with the given name does not exist.

  Error : Incorrect feature name.

getIncompatibleMeshInterfaces(cells: tuple[Cell] = ())

This method returns a sequence of face objects that are meshed with incompatible elements.

Parameters:

cells

A sequence of cell objects which will be used to search the incompatible faces.

Returns:

A python:sequence of Face objects.

getLength(edges: tuple[Edge])

This method returns the length of a given edge or group of edges.

Parameters:

edges

A sequence of Edge objects whose total length the method will calculate.

Returns:

length: python:float

A Float specifying the total length

getMassProperties(regions: str = '', relativeAccuracy: SymbolicConstantType = 'LOW', useMesh: BooleanType = False, specifyDensity: BooleanType = False, density: str = '', specifyThickness: BooleanType = False, thickness: str = '', miAboutCenterOfMass: BooleanType = True, miAboutPoint: tuple = ())

This method returns the mass properties of a part or region. Only beams, trusses, shells, solids, point, nonstructural mass, and rotary inertia elements are supported.

Parameters:

regions

A MeshElementArray, CellArray, FaceArray, or EdgeArray specifying the regions whose mass properties are to be queried. The whole part is queried by default.

relativeAccuracy

A SymbolicConstant specifying the relative accuracy for geometry computation. Possible values are LOW, MEDIUM and HIGH. The default value is LOW.

useMesh

A Boolean specifying whether the mesh should be used in the computation if the geometry is meshed. The default value is False.

specifyDensity

A Boolean specifying whether a user-specified density should be used in regions with density errors such as undefined material density. The default value is False.

density

A double value specifying the user-specified density value to be used in regions with density errors. The user-specified density should be greater than 0.

specifyThickness

A Boolean specifying whether a user-specified thickness should be used in regions with thickness errors such as undefined thickness. The default value is False.

thickness

A double value specifying the user-specified thickness value to be used in regions with thickness errors. The user-specified thickness should be greater than 0.

miAboutCenterOfMass

A Boolean specifying if the moments of inertia should be evaluated about the center of mass. The default value is True.

miAboutPoint

A tuple of three floats specifying the coordinates of the point about which to evaluate the moment of inertia. By default if the moments of inertia are not being evaluated about the center of mass, they will be evaluated about the origin.

Returns:

properties: python:dict

A Dictionary object with the following items: area: None or a Float specifying the sum of the area of the specified faces. The area is computed only for one side for shells. areaCentroid: None or a tuple of three Floats representing the coordinates of the area centroid. volume: None or a Float specifying the volume of the specified regions. volumeCentroid: None or a tuple of three Floats representing the coordinates of the volume centroid. massFromMassPerUnitSurfaceArea: None or a Float specifying the mass due to mass per unit surface area. mass: None or a Float specifying the mass of the specified regions. It is the total mass and includes mass from quantities such as mass per unit surface area. centerOfMass: None or a tuple of three Floats representing the coordinates of the center of mass. momentOfInertia: None or a tuple of six Floats representing the moments of inertia about the center of mass or about the point specified. warnings: A tuple of SymbolicConstants representing the problems encountered while computing the mass properties. Possible SymbolicConstants are: UNSUPPORTED_ENTITIES: Some unsupported entities exist in the specified region. The mass properties are computed only for beams, trusses, shells, solids, point and non-structural mass elements and rotary inertia elements. The mass properties are not computed for axisymmetric elements, springs, connectors, gaskets or any other elements. MISSING_THICKNESS: For some regions, the section definitions are missing thickness values. ZERO_THICKNESS: For some regions, the section definitions have a zero thickness value. VARIABLE_THICKNESS: The nodal thickness or field thickness specified for some regions has been ignored. NON_APPLICABLE_THICKNESS: For some regions, the thickness value is not applicable to the corresponding sections specified on the regions. MISSING_DENSITY: For some regions, the section definitions are missing material density values. MISSING_MATERIAL_DEFINITION: For some regions, the material definition is missing. ZERO_DENSITY: For some regions, the section definitions have a zero material density value. UNSUPPORTED_DENSITY: For some regions, either a negative material density or a temperature dependent density has been specified, or the material value is missing for one or more plies in the composite section. SHELL_OFFSETS: For shells, this method does not account for any offsets specified. MISSING_SECTION_DEFINITION: For some regions, the section definition is missing. UNSUPPORTED_SECTION_DEFINITION: The section definition provided for some regions is not supported. REINFORCEMENTS: This method does not account for any reinforcements specified on the model. SMEARED_PROPERTIES: For regions with composite section assignments, the density is smeared across the thickness. The volume centroid and center of mass computations for a composite shell use a lumped mass approach where the volume and mass is assumed to be lumped in the plane of the shell. As a result of these approximations the volume centroid, center of mass and moments of inertia may be slightly inaccurate for regions with composite section assignments. UNSUPPORTED_NON_STRUCTURAL_MASS_ENTITIES: This method does not account for any non-structural mass on wires. INCORRECT_MOMENT_OF_INERTIA: For geometry regions with non-structural mass per volume, the non-structural mass is assumed to be a point mass at the centroid of the regions. Thus, the moments of inertia may be inaccurate as the distribution of the non-structural mass is not accounted for. Use the mesh for accurately computing the moments of inertia. MISSING_BEAM_ORIENTATIONS: For some regions with beam section assignments, the beam section orientations are missing. UNSUPPORTED_BEAM_PROFILES: This method supports the Box, Pipe, Circular, Rectangular, Hexagonal, Trapezoidal, I, L, T, Arbitrary, and Tapered beam profiles. Any other beam profile is not supported. TAPERED_BEAM_MI: Moment of inertia calculations for tapered beams are not accurate. SUBSTRUCTURE_INCORRECT_PROPERTIES: The user assigned density and thickness is not considered for substructures. UNSUPPORTED_NON_STRUCTURAL_MASS_PROPORTIONAL: Non-structural mass with Mass Proportional distribution is not supported. Results are computed using Volume Proportional distribution.

getMeshControl(region: str, attribute: SymbolicConstantType)

This method returns a mesh control parameter for the specified region of a part.

Parameters:

region

A Cell, a Face, or an Edge object specifying the region to be queried.

attribute

A SymbolicConstant specifying the mesh control attribute to return. Possible values are:

• ELEM_SHAPE

• TECHNIQUE

• ALGORITHM

• MIN_TRANSITION

The return value depends on the value of the attribute argument. - If *attribute*=ELEM_SHAPE, the return value is a SymbolicConstant specifying the element shape used during meshing. Possible values are:

• LINE

• QUAD

• TRI

• QUAD_DOMINATED

• HEX

• TET

• WEDGE

• HEX_DOMINATED

• If *attribute*=TECHNIQUE, the return value is a SymbolicConstant specifying the

meshing technique to be used during meshing. Possible values are:

• FREE

• STRUCTURED

• SWEEP

• UNMESHABLE

Where UNMESHABLE indicates that no meshing technique is applicable with the currently assigned element shape. - If *attribute*=ALGORITHM, the return value is a SymbolicConstant specifying the meshing algorithm to be used during meshing. Possible values are:

• MEDIAL_AXIS

• ADVANCING_FRONT

• DEFAULT

• NON_DEFAULT

• NONE

Where NONE indicates that no algorithm is applicable. - If *attribute*=MIN_TRANSITION, the return value is a Boolean indicating whether minimum transition will be used during meshing. This option is applicable only to the following: - Free quadrilateral meshing or sweep hexahedral meshing with *algorithm*=MEDIAL_AXIS. - Structured quadrilateral meshing.

Returns:

The return value is a SymbolicConstant or a Boolean depending on the value of the

attribute argument.

Raises:

• TypeError

  The region cannot carry mesh controls.

getMeshStats(regions: tuple)

This method returns the mesh statistics for the given regions.

Parameters:

regions

A sequence or tuple of ConstrainedSketchGeometry regions for which mesh statistics should be returned.

Returns:

A MeshStats object.

getPartSeeds(attribute: SymbolicConstantType | float)

This method returns a part seed parameter for the part.

Parameters:

attribute

A SymbolicConstant specifying the type of part seed attribute to return. Possible values are: - SIZE - DEFAULT_SIZE - DEVIATION_FACTOR - MIN_SIZE_FACTOR The return value depends on the value of the attribute argument. - If *attribute*=SIZE, the return value is a Float specifying the assigned global element size. If part seeds are not defined, the return value is zero. - If *attribute*=DEFAULT_SIZE, the return value is a Float specifying a suggested default global element size based upon the part geometry. - If *attribute*=DEVIATION_FACTOR, the return value is a Float specifying the deviation factor h/Lh/L, where hh is the chordal deviation and LL is the element length. If part seeds are not defined, the return value is zero. - If *attribute*=MIN_SIZE_FACTOR, the return value is a Float specifying the size of the smallest allowable element as a fraction of the specified global element size. If part seeds are not defined, the return value is zero.

Returns:

The return value is a Float that depends on the value of the attribute argument.

Raises:

• An exception occurs if the part does not contain native geometry.

  Error: Part does not contain native geometry

getPerimeter(faces: tuple[Face])

This method returns the total perimeter of a given face or group of faces. All faces need to be on the same part. If the specified faces have shared edges, these edges are excluded from the computation, thus providing the length of the outer perimeter of the specified faces.

Parameters:

faces

A sequence of Face objects whose perimeter the method will calculate.

Returns:

perimeter: python:float

A Float specifying the perimeter

getUnmeshedRegions()

This method returns all geometric regions in the part that require a mesh for submitting an analysis but are either unmeshed or are meshed incompletely.

Returns:

A Region object, or None.

getVolume(cells: tuple[Cell], relativeAccuracy: float = 0)

This method returns the volume area of a given cell or group of cells.

Parameters:

cells

A sequence of Cell objects whose volume the method will calculate.

relativeAccuracy

A Float specifying the relative accuracy of the computation. The default value is 0.000001 (0.0001%).

Returns:

volume: python:float

A Float specifying the sum of the areas of the given faces

ignoreEntity(entities: tuple)

This method creates a virtual topology feature. Virtual topology allows unimportant entities to be ignored during mesh generation. You can combine two adjacent faces by specifying a common edge to ignore. Similarly, you can combine two adjacent edges by specifying a common vertex to ignore.

Parameters:

entities

A sequence of vertices and edges specifying the entities to be ignored during meshing.

Returns:

feature: Feature

A Feature object

isAlignedWithSketch()

This method checks if the normal of an analytical rigid surface part is aligned with that of its sketch.

Returns:

A Boolean value of python:True if the part is aligned with the sketch and python:False if it is not

aligned.

Raises:

• If the part is not an analytical rigid part:

  AbaqusException: Can only be used with analytical rigid parts.

isSetInternal(setName: str)

This command returns a flag indicating whether the Set is Internal.

Parameters:

setName

A string specifying the Set name.

isSuppressed()

This method queries the suppressed state of the feature.

Returns:

A Boolean value of python:True if the feature is suppressed and python:False if it is not suppressed.

isSurfaceInternal(surfaceName: str)

This command returns a flag indicating whether the Surface is Internal.

Parameters:

surfaceName

A string specifying the Surface name.

markSetInternal(setName: str, internalSet: BooleanType)

This command marks the given Set as internal or external.

Parameters:

setName

A string specifying the Set name.

internalSet

A Boolean specifying whether the Set should be marked as internal.

markSurfaceInternal(setName: str, internalSurface: BooleanType)

This command marks the given Surface as internal or external.

Parameters:

setName

A string specifying the Surface name.

internalSurface

A Boolean specifying whether the Surface should be marked as internal.

mergeElement(edge: str, elements: str)

Merge a selection of elements arranged in layers on an orphan mesh part into a single layer.

Parameters:

edge

A MeshEdge of one of the specified elements that serves as a reference edge to indicate the topological direction for merging elements. All specified elements must be reachable by topological navigation from this element edge, and the topological direction must be unambiguous.

elements

A MeshElementArray, a list of MeshElement objects, a Set, or a list of Set objects containing the elements to be included in the merge operation.

orientElements(pickedElements: tuple[MeshElement], referenceRegion: MeshFace)

This method orients the stack direction of elements in a continuum shell or gasket mesh.

Parameters:

pickedElements

A sequence of MeshElement objects specifying the elements to orient.

referenceRegion

A MeshFace object specifying a reference top face that indicates the desired orientation.

printAssignedSections()

This method prints information on each section that has been assigned to a region of the part.

projectEdgesOntoSketch(sketch: str, edges: tuple, constrainToBackground: BooleanType = True)

This method projects the selected edges of a part onto the specified ConstrainedSketch object. The edges appear as sketch geometry after projection. If the plane of projection is not parallel to the specified edge, the resultant sketch geometry may be of a different type. For example, a circular edge can be projected as an ellipse or a line depending on the angle of the plane of projection. By default, the projected edge will be constrained to the background geometry. You can remove this constraint by setting constrainToBackground to False.

Parameters:

sketch

The ConstrainedSketch object on which the edges are projected.

edges

A sequence of candidate edges to be projected onto the sketch.

constrainToBackground

A Boolean that determines whether the projected edges need to constrained to the background geometry. The default is True.

projectNode(nodes: tuple[MeshNode], projectionReference: str)

This method projects the given nodes onto a mesh entity, geometric entity, or a datum object. The nodes may belong to an orphan mesh part or to an Abaqus native mesh.

Parameters:

nodes

A sequence of MeshNode objects to be projected.

projectionReference

An object specifying the target for the node projection operation. The projectionReference can be any one of the following objects: MeshNode, MeshEdge, MeshFace, ConstrainedSketchVertex, Edge, Face, DatumPoint, DatumAxis, or DatumPlane.

projectReferencesOntoSketch(sketch: str, filter: ~abaqusConstants.SymbolicConstantType = 'ALL_EDGES', upToFeature: ~abaqus.Part.Feature.Feature = <abaqus.Part.Feature.Feature object>, edges: tuple = (), vertices: tuple = ())

This method projects the vertices of specified edges, and datum points from the part onto the specified ConstrainedSketch object. The vertices and datum points appear on the sketch as reference geometry.

Parameters:

sketch

The ConstrainedSketch object on which the edges, vertices, and datum points are projected.

filter

A SymbolicConstant specifying how to limit the amount of projection. Possible values are ALL_EDGES and COPLANAR_EDGES. If *filter*=COPLANAR_EDGES, edges that are coplanar to the sketching plane are the only candidates for projection. The default value is ALL_EDGES.

upToFeature

A Feature object specifying a marker in the feature-based history of the part. Abaqus/CAE projects onto the sketch only the part entities that were created before the feature specified by this marker. By default, part entities in features created before the sketch you are editing are candidates for projection.

edges

A sequence of candidate edges whose vertices need to be projected onto the sketch. By default, all edges specified by the filter argument are candidates for projection.

vertices

A sequence of candidate vertices to be projected onto the sketch. By default, all vertices are candidates for projection.

queryAttributes(printResults: BooleanType = 0)

This method prints the following information about a part:

• the name, modeling space, and analysis type; and

• whether twist is included (only available when the modeling space is axisymmetric and

the analysis type is deformable); and

• the number of vertices, edges, faces and cells if applicable.

Parameters:

printResults

A Boolean which specifies whether the above information is to be printed. The default value is True

Returns:

attributes: python:dict

A Dictionary object with string keys and integer values which returns the above information with the keys being numVertices, numEdges, numFaces, numCells, numWiredEdges, numShellFaces and numSolidFaces.

queryCachedStates()

This method displays the position of geometric states relative to the sequence of features in the part cache. The output is displayed in the message area.

queryDisjointPlyRegions()

This method provides a list of all composite plys in the current part which have disjoint regions.

queryGeometry(relativeAccuracy: float = 0, printResults: BooleanType = True)

This method prints the following information about a part:

• the name, modeling space, and analysis type;

• whether twist is included (only available when the modeling space is axisymmetric and

the analysis type is deformable);

• a 3D point representing the minimum of the part’s bounding box;

• a 3D point representing the maximum of the part’s bounding box;

• a 3D point representing the part’s centroid (only on 3D solid parts); and

• the volume (only on 3D solid parts).

Parameters:

relativeAccuracy

A Float specifying that the property computations should stop when the specified relative accuracy has been achieved. The default value is 0.000001 (0.0001%).

printResults

A Boolean which specifies whether the above information is to be printed. The default value is True.

Returns:

geometry: python:dict

A Dictionary object with string keys, which returns the above information with the keys being name, space, type, volume, centroid, category and boundingBox.

queryRegionsMissingSections()

This method returns all regions in the part that do not have a section assignment but require one for analysis.

Returns:

region: Region

A Region object, or None

redoMeshEdit()

This method executes the edit mesh or the bottom-up meshing operation most recently undone by the undoMeshEdit method on an part. A redo action must be currently available for the part. This implies that the user must have executed the undoMeshEdit method on the part and that the user has not subsequently executed any further edit mesh commands on the assembly. It also implies that the user provided a sufficient cache allowance to store the undo operation.

regenerate()

This method regenerates a part. When you modify features, it may be convenient to postpone regeneration until you make all your changes, since regeneration can be time consuming.

regenerationWarnings()

This method prints any regeneration warnings associated with the features.

removeElementSize()

This method removes the global element size from an orphan mesh part.

removeInvalidGeometry()

Removes all invalid entities from the part, leaving a valid part. This is not recorded as a feature in the feature list, therefore it should be used on parts that have a single feature (such as an imported part). Note:This may remove valid entities that are connected to invalid ones. You can identify invalid entities using the query toolset before using this command.

renumberElement(elements: tuple = (), startLabel: int | None = None, increment: int | None = None, offset: int | None = None, labels: str = '')

This method assigns new labels to orphan mesh elements.

Parameters:

elements

A MeshElementArray or a tuple or list of MeshElement objects, or a Set containing elements to be renumbered. If unspecified, all elements in the part will be renumbered.

startLabel

A positive Int specifying the new label for the first element in elements.

increment

A positive Int specifying the increment used for computation of new labels for all consecutive elements in elements.

offset

An Int by which existing labels of the specified elements will be offset.

labels

A list of labels for the specified elements. The length of this list must match the number of specified elements.

Raises:

• Renumbering is attempted on a native part:

  Error: Renumbering can be applied to orphan mesh parts only

• Renumbering data is specified incorrectly:

  Error: Either startLabel and increment or offset must be specified

• Renumbering will result in invalid labels:

  Error: Specified data will result in invalid labels

• Renumbering will result in conflicting labels:

  Error: Specified data will result in conflicting labels

renumberNode(nodes: tuple = (), startLabel: int | None = None, increment: int | None = None, offset: int | None = None, labels: str = '')

This method assigns new labels to orphan mesh nodes.

Parameters:

nodes

A MeshNodeArray or a tuple or list of MeshNode objects, or a Set containing nodes to be renumbered. If unspecified, all nodes in the part will be renumbered.

startLabel

A positive Int specifying the new label for the first node in nodes.

increment

A positive Int specifying the increment used for computation of new labels for all consecutive nodes in nodes.

offset

An Int by which existing labels of the specified nodes will be offset.

labels

A list of labels for the specified nodes. The length of this list must match the number of specified nodes.

Raises:

• Renumbering is attempted on a native part:

  Error: Renumbering can be applied to orphan mesh parts only

• Renumbering data is specified incorrectly:

  Error: Either startLabel and increment or offset must be specified

• Renumbering will result in invalid labels:

  Error: Specified data will result in invalid labels

• Renumbering will result in conflicting labels:

  Error: Specified data will result in conflicting labels

restore()

This method restores the parameters of all features in the assembly to the value they had before a failed regeneration. Use the restore method after a failed regeneration, followed by a regenerate command.

restoreIgnoredEntity(entities: tuple[IgnoredVertex])

This method restores vertices and edges that have been merged using a virtual topology feature.

Parameters:

entities

A sequence of IgnoredVertex objects and IgnoredEdge objects specifying the entities to be restored.

Returns:

feature: Feature

A Feature object

resume()

This method resumes suppressed features. Resuming a feature fully restores it to the part or assembly. You can resume the last feature you suppressed, all suppressed features, or just selected features. When you resume a child feature, Abaqus/CAE also resumes the parent features automatically.

resumeAllFeatures()

This method resumes all the suppressed features in the part.

resumeFeatures(featureNames: tuple)

This method resumes the specified suppressed features in the part.

Parameters:

featureNames

A tuple of names of features which are to be resumed.

resumeLastSetFeatures()

This method resumes the last set of features to be suppressed in the part.

saveGeometryCache()

This method caches the current geometry. Caching the current geometry improves regeneration performance.

seedEdgeByBias(biasMethod: SymbolicConstantType, end1Edges: tuple[Edge], end2Edges: tuple[Edge], centerEdges: tuple[Edge], endEdges: tuple[Edge], ratio: float, number: int, minSize: float, maxSize: float, constraint: SymbolicConstantType = 'FREE')

This method seeds the given edges nonuniformly using the specified number of elements and bias ratio or the specified minimum and maximum element sizes.

Parameters:

biasMethod

A SymbolicConstant specifying whether single- or double-biased seed distribution will be applied. If unspecified, single-biased seed distribution will be applied. Possible values are: - SINGLE: Single-biased seed distribution will be applied. - DOUBLE: Double-biased seed distribution will be applied.

end1Edges

A sequence of Edge objects specifying the edges to seed. The smallest elements will be positioned near the end where the normalized curve parameter=0.0. You must provide either the end1Edges or the end2Edges argument or both when *biasMethod*=SINGLE and omit both of them when *biasMethod*=DOUBLE.Note:You can determine which end is which by the order of the vertex indices returned by [getVertices()](https://help.3ds.com/2022/english/DSSIMULIA_Established/SIMACAEKERRefMap/simaker-c-edgepyc.htm?ContextScope=all#simaker-edgegetverticespyc).

end2Edges

A sequence of Edge objects specifying the edges to seed. The smallest elements will be positioned near the end where the normalized curve parameter=1.0.

centerEdges

A sequence of Edge objects specifying the edges to seed. The smallest elements will be positioned near edge center. You must provide either the centerEdges or the endEdges argument or both when *biasMethod*=DOUBLE and omit both of them when *biasMethod*=SINGLE.

endEdges

A sequence of Edge objects specifying the edges to seed. The smallest elements will be positioned near edge ends.

ratio

A Float specifying the ratio of the largest element to the smallest element. Possible values are 1.0 ≤≤ ratio ≤≤ 106.

number

An Int specifying the number of elements along each edge. Possible values are 1 ≤≤ number ≤≤ 104.

minSize

A Float specifying the desired smallest element size.

maxSize

A Float specifying the desired largest element size.Note:You must specify either the ratio and number or minSize and maxSize pair of arguments.

constraint

A SymbolicConstant specifying how closely the seeds must be matched by the mesh. The default value is FREE. If unspecified, the existing constraint will remain unchanged. Possible values are:

• FREE: The resulting mesh can be finer or coarser than the specified seeds.

• FINER: The resulting mesh can be finer than the specified seeds.

• FIXED: The seeds must be exactly matched by the mesh (only with respect to the number

of elements, not to the nodal positioning).

seedEdgeByNumber(edges: tuple[Edge], number: int, constraint: SymbolicConstantType = 'FREE')

This method seeds the given edges uniformly based on the number of elements along the edges.

Parameters:

edges

A sequence of Edge objects specifying the edges to seed.

number

An Int specifying the number of elements along each edge. Possible values are 1 ≤≤ number ≤≤ 104.

constraint

A SymbolicConstant specifying how closely the seeds must be matched by the mesh. The default value is FREE. If unspecified, the existing constraint will remain unchanged. Possible values are:

• FREE: The resulting mesh can be finer or coarser than the specified seeds.

• FINER: The resulting mesh can be finer than the specified seeds.

• FIXED: The seeds must be exactly matched by the mesh (only with respect to the number

of elements, not to the nodal positioning).

seedEdgeBySize(edges: tuple[Edge], size: float, deviationFactor: float | None = None, minSizeFactor: float | None = None, constraint: SymbolicConstantType = 'FREE')

This method seeds the given edges either uniformly or following edge curvature distribution, based on the desired element size.

Parameters:

edges

A sequence of Edge objects specifying the edges to seed.

size

A Float specifying the desired element size.

deviationFactor

A Float specifying the deviation factor h/Lh/L, where hh is the chordal deviation and LL is the element length.

minSizeFactor

A Float specifying the size of the smallest allowable element as a fraction of the specified global element size.

constraint

A SymbolicConstant specifying how closely the seeds must be matched by the mesh. The default value is FREE. If unspecified, the existing constraint will remain unchanged. Possible values are:

• FREE: The resulting mesh can be finer or coarser than the specified seeds.

• FINER: The resulting mesh can be finer than the specified seeds.

• FIXED: The seeds must be exactly matched by the mesh (only with respect to the number

of elements, not to the nodal positioning).

seedPart(size: float, deviationFactor: float | None = None, minSizeFactor: float | None = None, constraint: SymbolicConstantType = 'FREE')

This method assigns global edge seeds to the given parts.

Parameters:

size

A Float specifying the desired global element size for the edges.

deviationFactor

A Float specifying the deviation factor h/Lh/L, where hh is the chordal deviation and LL is the element length.

minSizeFactor

A Float specifying the size of the smallest allowable element as a fraction of the specified global element size.

constraint

A SymbolicConstant specifying how closely the seeds must be matched by the mesh. The default value is FREE. If unspecified, the existing constraint will remain unchanged. Possible values are:FREE: The resulting mesh can be finer or coarser than the specified seeds.FINER: The resulting mesh can be finer than the specified seeds.

setAssociatedCADPaths(partFile: str = '', rootFile: str = '')

This method sets the paths to the associated CAD part and root file. This method is only available if the part was imported from one of the supported CAD softwares using the Associative Import capability. The root file can be the assembly file or the part file, depending on the one that was imported. This method can be used to specify the new paths when the CAD data is moved to a different directory.

Parameters:

partFile

A String specifying the name of the associated CAD part file.

rootFile

A String specifying the name of the root associated CAD file. This can be the same as the part file or can be the assembly file, depending on the one that was imported.

setBoundaryLayerControls(regions: tuple[Cell], firstElemSize: float, growthFactor: float, numLayers: int, inactiveFaces: tuple[Face] = (), setName: str = '')

This method sets the control parameters for boundary layer mesh for the specified regions.

Parameters:

regions

A sequence of Cell objects specifying the regions for which to set the boundary layer mesh control parameters.

firstElemSize

A Float specifying the height of the first element layer off boundary. Possible values are 0.0 << firstElemSize ≤≤ 106.

growthFactor

A Float specifying the ratio of heights of any two consecutive element layers. Possible values are 1.0 ≤≤ growthFactor ≤≤ 10.0.

numLayers

An Int specifying the number of element layers to be generated. Possible values are 1 ≤≤ numLayers ≤≤ 104.

inactiveFaces

A sequence of Face objects specifying the faces where boundary layer should not be generated. By default, boundary layer mesh will be generated on all faces of the selected regions.

setName

A String specifying a unique name for a set that will contain boundary layer elements.

setElementSize(size: float)

This method sets the global element size for an orphan mesh part.

Parameters:

size

A Float specifying the desired element size.

setElementType(regions: tuple, elemTypes: tuple[ElemType])

This method assigns element types to the specified regions.

Parameters:

regions

A sequence of ConstrainedSketchGeometry regions or MeshElement objects, or a Set object containing either geometry regions or elements, specifying the regions to which element types are to be assigned.

elemTypes

A sequence of ElemType objects, one for each element shape applicable to the regions.Note:If an ElemType object has an UNKNOWN_*xxx* value for elemCode, its order will be deduced from the order of other valid ElemType objects within the same setElementType command. If no valid ElemType objects can be found, the order will remain unchanged.

Raises:

As a result of the element assignment, a region must have the same library, family, and

order for all its assigned element types. Otherwise, an exception will be thrown.

For example, suppose the Hex, Wedge, and Tet elements previously assigned to a cell are

all linear. The user now constructs an ElemType object with a quadratic Hex element and

includes only this object in the setElementType command. An exception will be thrown

because the Wedge and Tet elements will remain linear (i.e., As Is) and become

incompatible with the newly assigned quadratic Hex element.

setLogicalCorners(region: str, corners: str)

This method sets the logical corners for a mappable face region.

Parameters:

region

A Face region.

corners

Three, four, or five ConstrainedSketchVertex objects defining the logical corners for a given mappable face region.

setMeshControls(regions: tuple, elemShape: SymbolicConstantType | None = None, technique: SymbolicConstantType | None = None, algorithm: SymbolicConstantType | None = None, minTransition: BooleanType = 1, sizeGrowth: SymbolicConstantType | None = None, allowMapped: BooleanType = 0)

This method sets the mesh control parameters for the specified regions.

Parameters:

regions

A sequence of Face or Cell regions specifying the regions for which to set the mesh control parameters.

elemShape

A SymbolicConstant specifying the element shape to be used for meshing. The default value is QUAD for Face regions and HEX for Cell regions. If unspecified, the existing element shape will remain unchanged. Possible values are:

• QUAD: Quadrilateral mesh.

• QUAD_DOMINATED: Quadrilateral-dominated mesh.

• TRI: Triangular mesh.

• HEX: Hexahedral mesh.

• HEX_DOMINATED: Hex-dominated mesh.

• TET: Tetrahedral mesh.

• WEDGE: Wedge mesh.

technique

A SymbolicConstant specifying the mesh technique to be used. The default value is FREE for Face regions. For Cell regions the initial value depends on the geometry of the regions and can be STRUCTURED, SWEEP, or unmeshable. If unspecified, the existing mesh technique(s) will remain unchanged. Possible values are:

• FREE: Free mesh technique.

• STRUCTURED: Structured mesh technique.

• SWEEP: Sweep mesh technique.

• BOTTOM_UP: Bottom-up mesh technique. Only applicable for cell regions.

• SYSTEM_ASSIGN: Allow the system to assign a suitable technique. The actual technique

assigned can be STRUCTURED, SWEEP, or unmeshable.

algorithm

A SymbolicConstant specifying the algorithm used to generate the mesh for the specified regions. Possible values are MEDIAL_AXIS, ADVANCING_FRONT, and NON_DEFAULT. If unspecified, the existing value will remain unchanged. This option is applicable only to the following: - Free quadrilateral or quadrilateral-dominated meshing. In this case the possible values are MEDIAL_AXIS and ADVANCING_FRONT. - Sweep hexahedral or hexahedral-dominated meshing. In this case the possible values are MEDIAL_AXIS and ADVANCING_FRONT. - Free tetrahedral meshing. In this case the only possible value is NON_DEFAULT, and it indicates that the free tetrahedral-meshing technique available in Abaqus 6.4 or earlier will be used. If algorithm is not specified, the default

minTransition

A Boolean specifying whether minimum transition is to be applied. The default value is ON. If unspecified, the existing value will remain unchanged. This option is applicable only in the following cases: - Free quadrilateral meshing or hexahedral sweep meshing with *algorithm*=MEDIAL_AXIS. - Structured quadrilateral meshing.

sizeGrowth

A SymbolicConstant specifying element size growth to be applied when generating the interior of a tetrahedral mesh. Possible values are MODERATE and MAXIMUM. If unspecified, the existing value will remain unchanged. This option only applies to the default tetrahedral mesher.

allowMapped

A Boolean specifying whether mapped meshing can be used to replace the selected mesh technique. The allowMapped argument is applicable only in the following cases: - Free triangular meshing. - Free quadrilateral or quadrilateral-dominated meshing with algorithm*=ADVANCING_FRONT. - Hexahedral or hexahedral-dominated sweep meshing with *algorithm*=ADVANCING_FRONT. - Free tetrahedral meshing. *allowMapped*=True implies that mapped triangular meshing can be used on faces that bound three-dimensional *regions.

setSweepPath(region: str, edge: Edge, sense: SymbolicConstantType)

This method sets the sweep path for a sweepable region or the revolve path for a revolvable region.

Parameters:

region

A sweepable region.

edge

An Edge object specifying the sweep or revolve path.

sense

A SymbolicConstant specifying the sweep sense. The sense will affect only how gasket elements will be created; it will have no effect if gasket elements are not used. Possible values are FORWARD or REVERSE.If *sense*=FORWARD, the sense of the given edge’s underlying curve will be used.

setValues(*args, **kwargs)

This method modifies the Part object.

Raises:

RangeError

smoothNodes(nodes: tuple[MeshNode])

This method smooths the given nodes of a native mesh, moving them locally to a more optimal location that improves the quality of the mesh

Parameters:

nodes

A sequence of MeshNode objects or a Set object containing nodes.

splitElement(elements: tuple)

This method splits quadrilateral elements of an orphan mesh part or a Abaqus native mesh into triangular elements.

Parameters:

elements

A sequence of quadrilateral MeshElement objects specifying the elements to split. Each quadrilateral element is split into two triangular elements by the shorter diagonal.

splitMeshEdge(edge: str, parameter: float = 0)

This method splits an edge of a quadrilateral or triangular element of an orphan mesh part or an Abaqus native mesh.

Parameters:

edge

A single MeshEdge object specifying the element edge to split.

parameter

A Float specifying the normalized distance along edge at which to split. Possible values are 0.0 << parameter << 1.0. The default value is 0.5.

subdivideElement(elements: str = '', divisionNumber: int | None = None, face: ~abaqus.Mesh.MeshFace.MeshFace = <abaqus.Mesh.MeshFace.MeshFace object>, edge: ~abaqus.Mesh.MeshEdge.MeshEdge = <abaqus.Mesh.MeshEdge.MeshEdge object>)

Subdivide a selection of elements on an orphan mesh part in one or more directions.

Parameters:

elements

A MeshElementArray, a list of MeshElement objects, a Set, or a list of Set objects containing the elements to be subdivided. By default all the elements of the part are subdivided.

divisionNumber

An Int specifying the number of resulting elements for each input element in each direction of the subdivision. If face or edge are not specified, elements will be subdivided according to this number in all possible directions. Must be greater than one. Default is 2.

face

A MeshFace object that serves as a reference for indicating two topological directions for the subdivision operation. Must be a face of one of the specified elements, and all specified elements must be reachable by topological navigation from this element face. May not be combined with edge.

edge

A MeshEdge object that serves as a reference for indicating a single topological direction for the subdivision operation. Must be an edge of one of the specified elements, and all specified elements must be reachable by topological navigation from this element edge. May not be combined with face.

suppress()

This method suppresses features. Suppressing a feature is equivalent to temporarily removing the feature from the part or assembly. Suppressed features remain suppressed when you regenerate a part or assembly. You cannot suppress the base feature. In addition, if you suppress a parent feature, all of its child features are also suppressed automatically. Suppressed features can be restored with the resume command.

suppressFeatures(featureNames: tuple)

This method suppresses the given features.

Parameters:

featureNames

A tuple of names of features which are to be suppressed in the part.

swapMeshEdge(edge: str)

This method swaps the diagonal of two adjacent triangular elements of an orphan mesh part or an Abaqus native mesh.

Parameters:

edge

A single MeshEdge object specifying the element edge to swap.

undoMeshEdit()

This method undoes the most recent edit mesh or the bottom-up meshing operation on a part and restores the mesh to its previous state. An edit mesh undo action must be available for the part. This implies that prior to executing an edit mesh command on the part, the user enabled edit mesh undo with a sufficient cache allowance to store the edit mesh operation.

verifyMeshQuality(criterion: SymbolicConstantType, threshold: float | None = None, elemShape: SymbolicConstantType | None = None, regions: tuple = ())

This method tests the mesh quality of a part and returns poor-quality elements.

Parameters:

criterion

A SymbolicConstant specifying the criterion used for the quality check. Possible values are: - ANALYSIS_CHECKS When this criterion is specified Abaqus/CAE will invoke the element quality checks included with the input file processor for Abaqus/Standard and Abaqus/Explicit. - ANGULAR_DEVIATION The maximum amount (in degrees) that an element’s face corner angles deviate from the ideal angle. The ideal angle is 90° for quadrilateral element faces and 60° for triangular element faces. Elements with an angular deviation larger than the specified threshold will fail this test. - ASPECT_RATIO The ratio between the lengths of the longest and shortest edges of an element. Elements with an aspect ratio larger than the specified threshold will fail this test. - GEOM_DEVIATION_FACTOR The largest geometric deviation factor evaluated along any of the element edges associated with geometric edges or faces. The geometric deviation factor along an element edge is calculated by dividing the maximum gap between the element edge and its associated geometry by the length of the element edge. Elements with a geometric deviation factor larger than the specified threshold will fail this test. - LARGE_ANGLE The largest corner angle on any of an element’s faces. Elements with face angles larger than the specified threshold (in degrees) will fail this test. - LONGEST_EDGE The length of an element’s longest edge. Elements with an edge longer than the specified threshold will fail this test. - MAX_FREQUENCY An estimate of an element’s contribution to the initial maximum allowable frequency for Abaqus/Standard analyses. This calculation requires appropriate section assignments and material definitions. Elements whose maximum allowable frequency is smaller than the given value will fail this test. - SHAPE_FACTOR The shape factor for triangular and tetrahedral elements. This is the ratio between the element area or volume and the optimal element area or volume. Elements with a shape factor smaller than the specified threshold will fail this test. - SHORTEST_EDGE The length of an element’s shortest edge. Elements with an edge shorter than the specified threshold will fail this test. - SMALL_ANGLE The smallest corner angle on any of an element’s faces. Elements with face angles smaller than the given value (in degrees) will fail this test. - STABLE_TIME_INCREMENT An estimate of an element’s contribution to the initial maximum stable time increment for Abaqus/Explicit analyses. This calculation requires appropriate section assignments and material definitions. Elements that require a time increment smaller than the given value will fail this test.

threshold

A Float value used to determine low quality elements according to the specified criterion. This argument is ignored when the ANALYSIS_CHECKS criterion is used. For other criterion, if this argument is unspecified then no list of failed elements will be returned.

elemShape

A SymbolicConstant specifying an element shape for limiting the query. Possible values are LINE, QUAD, TRI, HEX, WEDGE, and TET.

regions

A sequence of Region or MeshElement objects. If you do not specify the regions argument, the entire part mesh is considered.

Returns:

A Dictionary object containing values for some number of the following keys:

failedElements, warningElements, naElements (sequences of MeshElement objects);

numElements (Int); average, worst (Float); worstElement (MeshElement object) .

wrapMesh(radius: float)

This method wraps a planar orphan mesh part about the Z-axis.

Parameters:

radius

A Float specifying the radius of the cylinder about which the part is to be wrapped. The wrapping procedure will relocate a node at point (xx, yy) on the planar mesh to (x,θ,zx,θ,z), where rr is the specified radius, θθ = xrxr, and zz=yy.

writeAcisFile(fileName: str, version: float | None = None)

This method exports the geometry of the part to a named file in ACIS format.

Parameters:

fileName

A String specifying the name of the file to which to write.

version

A Float specifying the ACIS version. For example, the Float 12.0 corresponds to ACIS Version 12.0. The default value is the current version of ACIS.

Raises:

• If the part is an orphan mesh part:

  Cannot export orphan mesh parts to ACIS.

writeCADParameters(paramFile: str, modifiedParams: tuple = (), updatePaths: str = '')

This method writes the parameters that were imported from the CAD system to a parameter file.

Parameters:

paramFile

A String specifying the parameter file name.

modifiedParams

A tuple of tuples each containing the part name, the parameter name, and the modified parameter value. Default is an empty tuple.

updatePaths

A Bool specifying whether to update the path of the CAD model file specified in the parameterFile to the current directory, if the CAD model is present in the current directory.

writeIgesFile(fileName: str, flavor: SymbolicConstantType)

This method exports the geometry of the part to a named file in IGES format.

Parameters:

fileName

A String specifying the name of the file to which to write.

flavor

A SymbolicConstant specifying a particular flavor of IGES. Possible values are STANDARD, AUTOCAD, SOLIDWORKS, JAMA, and MSBO.

Raises:

• If the part is an orphan mesh part:

  Cannot export orphan mesh parts to IGES.

writeStepFile(fileName: str)

This method exports the geometry of the part to a named file in STEP format.

Parameters:

fileName

A String specifying the name of the file to which to write.

Raises:

• If the part contains no geometry:

  Parterror: Cannot export orphan mesh parts to STEP.

writeVdaFile(fileName: str)

This method exports the geometry of the part to a named file in VDA-FS format.

Parameters:

fileName

A String specifying the name of the file to which to write.

Raises:

• If the part is an orphan mesh part:

  Cannot export orphan mesh parts to VDA-FS.

AcisFile

class AcisFile

The AcisFile object is a file object used to open ACIS-, STEP-, and IGES-format files.

Notes

This object can be accessed by:

import part

Attributes:

numberOfParts: int

An Int specifying the number of parts in the object.

Methods

openAcis(fileName[, scaleFromFile])	This method creates an AcisFile object from a file containing ACIS-format geometry.
openCatia(fileName[, topology, ...])	This method creates an AcisFile object from a file containing V5-format geometry.
openEnf(fileName, fileType[, topology, ...])	This method creates an AcisFile object from a file containing Elysium Neutral File-format geometry that was created by CATIA V5, I-DEAS, or Pro/ENGINEER.
openIges(fileName[, trimCurve, ...])	This method creates an AcisFile object from a file containing IGES-format geometry.
openParasolid(fileName[, topology])	This method creates an AcisFile object from a file containing Parasolid-format geometry.
openSolidworks(fileName[, topology])	This method creates an AcisFile object from a file containing Solidworks format geometry.
openStep(fileName[, scale])	This method creates an AcisFile object from a file containing STEP-format geometry.
openVda(fileName)	This method creates an AcisFile object from a file containing VDA-FS-format geometry.
writeAcisFile(fileName[, version])	This method exports the assembly to a named file in ACIS format.

openAcis(fileName: str, scaleFromFile: BooleanType = 0)

This method creates an AcisFile object from a file containing ACIS-format geometry. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the ACIS file to open.

scaleFromFile

A Boolean specifying whether to scale, rotate, and translate the part using the transform read from the ACIS file. The default value is OFF.

Returns:

An AcisFile object.

Raises:

• File is from a newer version of ACIS than the CAE kernel.

  Texterror: ACIS File version exceeds Kernel.

• The data in the ACIS file are corrupted.

  Texterror: Failed to read ACIS file.

Notes

This function can be accessed by:

mdb.openAcis

openCatia(fileName: str, topology: SymbolicConstantType | None = None, convertUnits: SymbolicConstantType = 0, combineBodies: BooleanType = 0)

This method creates an AcisFile object from a file containing V5-format geometry. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the CATIA file to open.

topology

A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If *topology*=SOLID, Abaqus/CAE attempts to attach cells to create a solid. If *topology*=SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID .

convertUnits

A SymbolicConstant specifying whether the original units should be retained. Possible values are ON and OFF. The default value is OFF.

combineBodies

A Boolean specifying whether to combine the bodies in the CATPart file. If the bodies to be combined touch or overlap, invalid entities would result. For CATProduct files, this option will be ignored.

Returns:

An AcisFile object.

Notes

This function can be accessed by:

mdb.openAcis

openEnf(fileName: str, fileType: str, topology: SymbolicConstantType = 'SOLID', convertUnits: BooleanType = 0)

This method creates an AcisFile object from a file containing Elysium Neutral File-format geometry that was created by CATIA V5, I-DEAS, or Pro/ENGINEER. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the Elysium Neutral File that was created by I-DEAS, Pro/ENGINEER, or CATIA V5.

fileType

A String specifying the type of CAD system that created the file. Possible values are “ideas”, “proe”, or “catiav5” or a combination similar to “proe/ideas/catiav5” if the type is unknown.

topology

A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If *topology*=SOLID, Abaqus/CAE attempts to attach cells to create a solid. If *topology*=SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID.

convertUnits

A Boolean specifying if the dimensions of the part should be converted to millimeters. The default value is OFF.

Returns:

An AcisFile object.

Notes

This function can be accessed by:

mdb.openAcis

openIges(fileName: str, trimCurve: SymbolicConstantType = 'DEFAULT', scaleFromFile: SymbolicConstantType = 0, msbo: BooleanType = False, includedLayers: tuple = (), topology: SymbolicConstantType = 'SOLID', uniteWires: SymbolicConstantType = 1)

This method creates an AcisFile object from a file containing IGES-format geometry. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the IGES file to open.

trimCurve

A SymbolicConstant specifying the method used to define the trim curves that bound parametric surfaces. Possible values are:DEFAULT, use either of the following as specified by the contents of the IGES file.PARAMETRIC_DATA, use the parameter space of the surface being trimmed.THREED_DATA, use real space—the coordinate system of the part along with an indication that the trim curve lies on the parametric surface.The default value is DEFAULT.

scaleFromFile

A SymbolicConstant specifying whether the imported geometry needs to be scaled using the units information available in the IGES file. Possible values are ON and OFF. The default value is OFF. When the argument is set to ON, the geometry is scaled to millimeters with respect to the unit system specified in the IGES file.

msbo

A Boolean specifying if the IGES file contains MSBO (Manifold Solid B-Rep Object) entities. The default value is False.

includedLayers

A sequence of Ints specifying the levels or layers of entities that will be translated from the IGES file to build the part. The default is to include all the layers.

topology

A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If *topology*=SOLID, Abaqus/CAE attempts to attach cells to create a solid. If *topology*=SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID.

uniteWires

A SymbolicConstant specifying whether the imported wires need to be united or not. Possible values are ON and OFF. The default value is ON. When importing a sketch, this value is set to OFF.

Returns:

An AcisFile object.

Raises:

• The data in the IGES file are corrupted.

  Texterror: Failed to read IGES file.

Notes

This function can be accessed by:

mdb.openAcis

openParasolid(fileName: str, topology: SymbolicConstantType = 'SOLID')

This method creates an AcisFile object from a file containing Parasolid-format geometry. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the Parasolid file to open.

topology

A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If *topology*=SOLID, Abaqus/CAE attempts to attach cells to create a solid. If *topology*=SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID.

Returns:

An AcisFile object.

Notes

This function can be accessed by:

mdb.openAcis

openSolidworks(fileName: str, topology: SymbolicConstantType = 'SOLID')

This method creates an AcisFile object from a file containing Solidworks format geometry. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the Solidworks file to open.

topology

A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID, SHELL, and WIRE. If *topology*=SOLID, Abaqus/CAE attempts to attach cells to create a solid entity. If *topology*=SHELL, Abaqus/CAE builds the body as a shell entity, not as a solid entity. The default value is SOLID.

Returns:

An AcisFile object.

Raises:

• The data in the Solidworks file are corrupted.

  Texterror: Failed to read Solidworks file.

Notes

This function can be accessed by:

mdb.openAcis

openStep(fileName: str, scale: float = 1)

This method creates an AcisFile object from a file containing STEP-format geometry. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the STEP file to open.

scale

A Float specifying the scaling factor to apply to the imported geometric entities. The default value is 1.0.

Returns:

An AcisFile object.

Raises:

• The data in the STEP file are corrupted.

  Texterror: Failed to read STEP file.

Notes

This function can be accessed by:

mdb.openAcis

openVda(fileName: str)

This method creates an AcisFile object from a file containing VDA-FS-format geometry. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the VDA-FS file to open.

Returns:

An AcisFile object.

Raises:

• The data in the VDA-FS file are corrupted.

  Texterror: Failed to read VDA file.

Notes

This function can be accessed by:

mdb.openAcis

writeAcisFile(fileName: str, version: float | None = None)

This method exports the assembly to a named file in ACIS format.

Parameters:

fileName

A String specifying the name of the file to which to write.

version

A Float specifying the ACIS version. For example, the Float 12.0 corresponds to ACIS Version 12.0. The default value is the current version of ACIS.

AcisMdb

class AcisMdb(pathName: str = '')

The Mdb object is the high-level Abaqus model database. A model database stores models and analysis controls.

Notes

This object can be accessed by:

mdb

Methods

openAcis(fileName[, scaleFromFile])	This method creates an AcisFile object from a file containing ACIS-format geometry.
openCatia(fileName[, topology, ...])	This method creates an AcisFile object from a file containing V5-format geometry.
openEnf(fileName, fileType[, topology, ...])	This method creates an AcisFile object from a file containing Elysium Neutral File-format geometry that was created by CATIA V5, I-DEAS, or Pro/ENGINEER.
openIges(fileName[, trimCurve, ...])	This method creates an AcisFile object from a file containing IGES-format geometry.
openParasolid(fileName[, topology])	This method creates an AcisFile object from a file containing Parasolid-format geometry.
openSolidworks(fileName[, topology])	This method creates an AcisFile object from a file containing Solidworks format geometry.
openStep(fileName[, scale])	This method creates an AcisFile object from a file containing STEP-format geometry.
openVda(fileName)	This method creates an AcisFile object from a file containing VDA-FS-format geometry.

static openAcis(fileName: str, scaleFromFile: BooleanType = 0)

This method creates an AcisFile object from a file containing ACIS-format geometry. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the ACIS file to open.

scaleFromFile

A Boolean specifying whether to scale, rotate, and translate the part using the transform read from the ACIS file. The default value is OFF.

Returns:

An AcisFile object.

Raises:

• File is from a newer version of ACIS than the CAE kernel.

  Texterror: ACIS File version exceeds Kernel.

• The data in the ACIS file are corrupted.

  Texterror: Failed to read ACIS file.

Notes

This function can be accessed by:

mdb.openAcis

static openCatia(fileName: str, topology: SymbolicConstantType | None = None, convertUnits: SymbolicConstantType = 0, combineBodies: BooleanType = 0)

This method creates an AcisFile object from a file containing V5-format geometry. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the CATIA file to open.

topology

A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If *topology*=SOLID, Abaqus/CAE attempts to attach cells to create a solid. If *topology*=SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID .

convertUnits

A SymbolicConstant specifying whether the original units should be retained. Possible values are ON and OFF. The default value is OFF.

combineBodies

A Boolean specifying whether to combine the bodies in the CATPart file. If the bodies to be combined touch or overlap, invalid entities would result. For CATProduct files, this option will be ignored.

Returns:

An AcisFile object.

Notes

This function can be accessed by:

mdb.openCatia

static openEnf(fileName: str, fileType: str, topology: SymbolicConstantType = 'SOLID', convertUnits: BooleanType = 0)

This method creates an AcisFile object from a file containing Elysium Neutral File-format geometry that was created by CATIA V5, I-DEAS, or Pro/ENGINEER. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the Elysium Neutral File that was created by I-DEAS, Pro/ENGINEER, or CATIA V5.

fileType

A String specifying the type of CAD system that created the file. Possible values are “ideas”, “proe”, or “catiav5” or a combination similar to “proe/ideas/catiav5” if the type is unknown.

topology

A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If *topology*=SOLID, Abaqus/CAE attempts to attach cells to create a solid. If *topology*=SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID.

convertUnits

A Boolean specifying if the dimensions of the part should be converted to millimeters. The default value is OFF.

Returns:

An AcisFile object.

Notes

This function can be accessed by:

mdb.openEnf

static openIges(fileName: str, trimCurve: SymbolicConstantType = 'DEFAULT', scaleFromFile: SymbolicConstantType = 0, msbo: BooleanType = False, includedLayers: tuple = (), topology: SymbolicConstantType = 'SOLID', uniteWires: SymbolicConstantType = 1)

This method creates an AcisFile object from a file containing IGES-format geometry. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the IGES file to open.

trimCurve

A SymbolicConstant specifying the method used to define the trim curves that bound parametric surfaces. Possible values are:DEFAULT, use either of the following as specified by the contents of the IGES file.PARAMETRIC_DATA, use the parameter space of the surface being trimmed.THREED_DATA, use real space—the coordinate system of the part along with an indication that the trim curve lies on the parametric surface.The default value is DEFAULT.

scaleFromFile

A SymbolicConstant specifying whether the imported geometry needs to be scaled using the units information available in the IGES file. Possible values are ON and OFF. The default value is OFF. When the argument is set to ON, the geometry is scaled to millimeters with respect to the unit system specified in the IGES file.

msbo

A Boolean specifying if the IGES file contains MSBO (Manifold Solid B-Rep Object) entities. The default value is False.

includedLayers

A sequence of Ints specifying the levels or layers of entities that will be translated from the IGES file to build the part. The default is to include all the layers.

topology

A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If *topology*=SOLID, Abaqus/CAE attempts to attach cells to create a solid. If *topology*=SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID.

uniteWires

A SymbolicConstant specifying whether the imported wires need to be united or not. Possible values are ON and OFF. The default value is ON. When importing a sketch, this value is set to OFF.

Returns:

An AcisFile object.

Raises:

• The data in the IGES file are corrupted.

  Texterror: Failed to read IGES file.

Notes

This function can be accessed by:

mdb.openIges

static openParasolid(fileName: str, topology: SymbolicConstantType = 'SOLID')

This method creates an AcisFile object from a file containing Parasolid-format geometry. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the Parasolid file to open.

topology

A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If *topology*=SOLID, Abaqus/CAE attempts to attach cells to create a solid. If *topology*=SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID.

Returns:

An AcisFile object.

Notes

This function can be accessed by:

mdb.openParasolid

static openSolidworks(fileName: str, topology: SymbolicConstantType = 'SOLID')

This method creates an AcisFile object from a file containing Solidworks format geometry. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the Solidworks file to open.

topology

A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID, SHELL, and WIRE. If *topology*=SOLID, Abaqus/CAE attempts to attach cells to create a solid entity. If *topology*=SHELL, Abaqus/CAE builds the body as a shell entity, not as a solid entity. The default value is SOLID.

Returns:

An AcisFile object.

Raises:

• The data in the Solidworks file are corrupted.

  Texterror: Failed to read Solidworks file.

Notes

This function can be accessed by:

openSolidworks

static openStep(fileName: str, scale: float = 1)

This method creates an AcisFile object from a file containing STEP-format geometry. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the STEP file to open.

scale

A Float specifying the scaling factor to apply to the imported geometric entities. The default value is 1.0.

Returns:

An AcisFile object.

Raises:

• The data in the STEP file are corrupted.

  Texterror: Failed to read STEP file.

Notes

This function can be accessed by:

mdb.openStep

static openVda(fileName: str)

This method creates an AcisFile object from a file containing VDA-FS-format geometry. This object is subsequently used by the PartFromGeometryFile method.

Parameters:

fileName

A String specifying the path to the VDA-FS file to open.

Returns:

An AcisFile object.

Raises:

• The data in the VDA-FS file are corrupted.

  Texterror: Failed to read VDA file.

Notes

This function can be accessed by:

mdb.openVda

Feature

class Feature

The following commands operate on Feature objects. For more information about the Feature object, see Feature object.

Notes

This object can be accessed by:

import part

Methods

AddCells(faceList[, flipped])	This method tries to convert a shell entity to a solid entity.
AnalyticRigidSurf2DPlanar(sketch)	This method creates a first Feature object for an analytical rigid surface by creating a planar wire from the given ConstrainedSketch object.
AnalyticRigidSurfExtrude(sketch[, depth])	This method creates a first Feature object for an analytical rigid surface by extruding the given ConstrainedSketch object by the given depth, creating a surface.
AnalyticRigidSurfRevolve(sketch)	This method creates a first Feature object for an analytical rigid surface by revolving the given ConstrainedSketch object by 360° about the Y-axis.
AssignMidsurfaceRegion(cellList)	This method assign a mid-surface property to sequence of Cell objects.
AutoRepair()	This method carries out a sequence of geometry repair operations if it contains invalid entities.
BaseShell(sketch)	This method creates a first Feature object by creating a planar shell from the given ConstrainedSketch object.
BaseShellExtrude(sketch, depth[, ...])	This method creates a first Feature object by extruding the given ConstrainedSketch object by the given depth, creating a shell.
BaseShellRevolve(sketch, angle[, pitch, ...])	This method creates a first Feature object by revolving the given ConstrainedSketch object by the given angle, creating a shell.
BaseShellSweep(sketch, path)	This method creates a first Feature object by sweeping the given section ConstrainedSketch object along the path defined by the path ConstrainedSketch object, creating a shell.
BaseSolidExtrude(sketch, depth[, ...])	This method creates a first Feature object by extruding the given ConstrainedSketch object by the given depth, creating a solid.
BaseSolidRevolve(sketch, angle[, pitch, ...])	This method creates a first Feature object by revolving the given ConstrainedSketch object by the given angle, creating a solid.
BaseSolidSweep(sketch, path)	This method creates a first Feature object by sweeping the given profile ConstrainedSketch object along the path defined by the path ConstrainedSketch object, creating a solid.
BaseWire(sketch)	This method creates a first Feature object by creating a planar wire from the given ConstrainedSketch object.
BlendFaces(side1, side2[, method, path])	This method creates a Feature object by creating new faces that blends two sets of faces.
Chamfer(length, edgeList)	This method creates an additional Feature object by chamfering the given list of edges with a given length.
ConvertToAnalytical()	This method attempts to change entities into a simpler form that will speed up processing and make entities available during feature operations.
ConvertToPrecise([method])	This method attempts to change imprecise entities so that the geometry becomes precise.
CoverEdges(edgeList[, tryAnalytical])	This method generates a face using the given edges as the face's boundaries.
Cut(sketchPlane, sketchPlaneSide, ...[, ...])	This method creates an additional Feature object by cutting a hole using the given ConstrainedSketch object.
CutExtrude(sketchPlane, sketchPlaneSide, ...)	This method creates an additional Feature object by extruding the given ConstrainedSketch object by the given depth and cutting away material in the solid and shell regions of the part.
CutLoft(loftsections[, startCondition, ...])	This method creates an additional Feature object by lofting between the given sections and cutting away material from the part.
CutRevolve(sketchPlane, sketchPlaneSide, ...)	This method creates an additional Feature object by revolving the given ConstrainedSketch object by the given angle and cutting away material from the part.
CutSweep(path, profile[, pathPlane, ...])	This method creates an additional Feature object by sweeping the given ConstrainedSketch object along a path which may be a ConstrainedSketch or a sequence of Edge objects and cutting away material from the part.
ExtendFaces([faces, extendAlong, distance, ...])	This method extends faces along its free edges by offsetting the external edges along the surfaces.
FaceFromElementFaces(elementFaces[, stitch, ...])	This method creates a geometry face from a collection of orphan element faces.
HoleBlindFromEdges(plane, planeSide, ...)	This method creates an additional Feature object by creating a circular blind hole of the given diameter and depth and cutting away material in the solid and shell regions of the part.
HoleFromEdges(diameter, edge1, distance1, ...)	This method creates an additional Feature object by creating a circular hole of the given diameter in a 2D planar part and cutting away material in the shell and wire regions of the part.
HoleThruAllFromEdges(plane, planeSide, ...)	This method creates an additional Feature object by creating a circular through hole of the given diameter and cutting away material in the solid and shell regions of the part.
MergeEdges([edgeList, extendSelection])	This method merges edges either by extending the user selection or using only the selected edges.
Mirror(mirrorPlane, keepOriginal[, ...])	This method mirrors existing part geometry across a plane to create new geometry.
OffsetFaces(faceList[, distance, ...])	This method creates new faces by offsetting existing faces.
RemoveCells(cellList)	This method converts a solid entity to a shell entity.
RemoveFaces(faceList[, deleteCells])	This method removes faces from a solid entity or from a shell entity.
RemoveFacesAndStitch(faceList)	This method removes faces from a solid entity and attempts to close the resulting gap by extending the neighboring faces of the solid.
RemoveRedundantEntities([vertexList, ...])	This method removes redundant edges and vertices from a solid or a shell entity.
RepairFaceNormals([faceList])	This method works on the entire part or a sequence of shell faces.
RepairInvalidEdges(edgeList)	This method repairs invalid edges.
RepairSliver(face, point1, point2[, ...])	This method repairs the selected sliver from the selected face.
RepairSmallEdges(edgeList[, toleranceChecks])	This method repairs small edges.
RepairSmallFaces(faceList[, toleranceChecks])	This method repairs small faces.
ReplaceFaces(faceList[, stitch])	This method replaces the selected faces with a single face.
Round(radius, edgeList, vertexList)	This method creates an additional Feature object by rounding (filleting) the given list of entities with the given radius.
Shell(sketchPlane, sketchPlaneSide, ...[, ...])	This method creates an additional Feature object by creating a planar shell from the given ConstrainedSketch object.
ShellExtrude(sketchPlane, sketchPlaneSide, ...)	This method creates an additional Feature object by extruding the given ConstrainedSketch object by the given depth, creating a shell protrusion.
ShellLoft(loftsections[, startCondition, ...])	This method creates an additional Feature object by lofting between the given sections and adding shell faces to the part.
ShellRevolve(sketchPlane, sketchPlaneSide, ...)	This method creates an additional Feature object by revolving the given ConstrainedSketch object by the given angle, creating a shell protrusion.
ShellSweep(path, profile[, pathPlane, ...])	This method creates an additional Feature object by sweeping the given ConstrainedSketch object or a sequence of Edge objects along a path which may be a ConstrainedSketch or a sequence of Edge objects, creating a shell swept protrusion.
SolidExtrude(sketchPlane, sketchPlaneSide, ...)	This method creates an additional Feature object by extruding the given ConstrainedSketch object by the given depth, creating a solid protrusion.
SolidLoft(loftsections[, startCondition, ...])	This method creates an additional Feature object by lofting between the given sections and adding material to the part.
SolidRevolve(sketchPlane, sketchPlaneSide, ...)	This method creates an additional Feature object by revolving the given ConstrainedSketch object by the given angle, creating a solid protrusion.
SolidSweep(path, profile[, pathPlane, ...])	This method creates an additional Feature object by sweeping the given ConstrainedSketch object or a Face object along a path which may be a ConstrainedSketch or a sequence of Edge objects, creating a solid swept protrusion.
Stitch([edgeList, stitchTolerance])	This method attempts to create a valid part by binding together free and imprecise edges of all the faces of a part.
Wire(sketchPlane, sketchPlaneSide, ...[, ...])	This method creates an additional Feature object by creating a planar wire from the given ConstrainedSketch object.
WireFromEdge(edgeList)	This method creates an additional Feature object by creating a Wire by selecting one or more Edge objects of a Solid or Shell part.
WirePolyLine(points[, mergeType, meshable])	This method creates an additional Feature object by creating a polyline wire that passes through a sequence of given points.
WireSpline(points[, mergeType, ...])	This method creates an additional Feature object by creating a spline wire that passes through a sequence of given points.

AddCells(faceList: tuple[Face], flipped: BooleanType = 0)

This method tries to convert a shell entity to a solid entity. The conversion is not always successful.

Parameters:

faceList

A sequence of Face objects specifying the faces bounding the cell to add.

flipped

A Boolean specifying the direction of feature creation. The possible values are True and False. The default is True indicating that the direction is opposite to the face normal. When multiple faces are selected, Abaqus attempts to create cells on both sides of the selected faces and ignores the flipped argument.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

AnalyticRigidSurf2DPlanar(sketch: ConstrainedSketch)

This method creates a first Feature object for an analytical rigid surface by creating a planar wire from the given ConstrainedSketch object.

Parameters:

sketch

A ConstrainedSketch object specifying the planar wire.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

AnalyticRigidSurfExtrude(sketch: ConstrainedSketch, depth: float = 1)

This method creates a first Feature object for an analytical rigid surface by extruding the given ConstrainedSketch object by the given depth, creating a surface.

Parameters:

sketch

A ConstrainedSketch object specifying the planar wire.

depth

A Float specifying the extrusion depth. The default value is 1.0.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

AnalyticRigidSurfRevolve(sketch: ConstrainedSketch)

This method creates a first Feature object for an analytical rigid surface by revolving the given ConstrainedSketch object by 360° about the Y-axis.

Parameters:

sketch

A ConstrainedSketch object specifying the surface to be revolved.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

AssignMidsurfaceRegion(cellList: tuple[Cell])

This method assign a mid-surface property to sequence of Cell objects. If a reference representation of the part does not exist, it creates one. It also copies the cells to the reference representation and deletes the cells from the active representation of the part.

Parameters:

cellList

A sequence of Cell objects specifying the regions that will be used for mid-surface construction. These regions will be copied to the reference representation of the part.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

AutoRepair()

This method carries out a sequence of geometry repair operations if it contains invalid entities. It is expected to improve the geometry, but it does not guarantee that the number of invalid entities will decrease. In some cases, it can also increase the number of invalid entities. Since a number of geometry repair operations and validity checks are performed, it could be a slow operation depending on the complexity of the geometry.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseShell(sketch: ConstrainedSketch)

This method creates a first Feature object by creating a planar shell from the given ConstrainedSketch object. The ConstrainedSketch object must define a closed profile.

Parameters:

sketch

A ConstrainedSketch object specifying the planar shell.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseShellExtrude(sketch: ConstrainedSketch, depth: float, draftAngle: float | None = None, pitch: float | None = None)

This method creates a first Feature object by extruding the given ConstrainedSketch object by the given depth, creating a shell. The ConstrainedSketch object can define either an open or closed profile.

Parameters:

sketch

A ConstrainedSketch object specifying the shape to be extruded.

depth

A Float specifying the extrusion depth. Possible values are Floats > 0.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

Returns:

A Feature object.

Raises:

RangeError

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseShellRevolve(sketch: ConstrainedSketch, angle: float, pitch: float | None = None, flipRevolveDirection: BooleanType = 0, flipPitchDirection: BooleanType = 0, moveSketchNormalToPath: BooleanType = 0)

This method creates a first Feature object by revolving the given ConstrainedSketch object by the given angle, creating a shell. The ConstrainedSketch object can define either an open or closed profile and an axis of revolution. The axis is defined by a single construction line.

Parameters:

sketch

A ConstrainedSketch object specifying the shape to be revolved.

angle

A Float specifying the revolve angle in degrees. Possible values are 0 ≤≤ angle ≤≤ 360.Note:If pitch >> 0, there is no upper limit for angle.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤≤ pitch ≤≤ 105. The default value, 0, implies a normal revolve.

flipRevolveDirection

A Boolean specifying whether to override the direction of feature creation. If *flipRevolveDirection*=OFF, the default direction of revolution is used. If *flipRevolveDirection*=ON, the revolve direction is reversed. The default value is OFF.

flipPitchDirection

A Boolean specifying whether to override the direction of translation. If *flipPitchDirection*=OFF, the direction of translation is given by the direction of the revolve axis. If *flipPitchDirection*=ON, the translation direction is reversed. The default value is OFF.

moveSketchNormalToPath

A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath*=OFF, the sketch plane remains parallel to the revolve axis. If *moveSketchNormalToPath*=ON, the sketch is moved to match the angle created by the *pitch before being revolved. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseShellSweep(sketch: ConstrainedSketch, path: ConstrainedSketch)

This method creates a first Feature object by sweeping the given section ConstrainedSketch object along the path defined by the path ConstrainedSketch object, creating a shell. The ConstrainedSketch object can define either an open or closed profile. The origin of the profile sketch is positioned at the start of the sweep path and swept perpendicular to the path. No checks are made for self-intersection.

Parameters:

sketch

A ConstrainedSketch object specifying the section to be swept.

path

A ConstrainedSketch object specifying the path of the sweep.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseSolidExtrude(sketch: ConstrainedSketch, depth: float, draftAngle: float | None = None, pitch: float | None = None)

This method creates a first Feature object by extruding the given ConstrainedSketch object by the given depth, creating a solid. The ConstrainedSketch object must define a closed profile.

Parameters:

sketch

A ConstrainedSketch object specifying the plane shape to be extruded.

depth

A Float specifying the extrusion depth. Possible values are 10–5 ≤≤ depth ≤≤ 105.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

Returns:

A Feature object.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseSolidRevolve(sketch: ConstrainedSketch, angle: float, pitch: float | None = None, flipRevolveDirection: BooleanType = 0, flipPitchDirection: BooleanType = 0, moveSketchNormalToPath: BooleanType = 0)

This method creates a first Feature object by revolving the given ConstrainedSketch object by the given angle, creating a solid. The ConstrainedSketch object must define a closed profile and an axis of revolution. The axis is defined by a single construction line.

Parameters:

sketch

A ConstrainedSketch object specifying the shape to be revolved.

angle

A Float specifying the revolve angle in degrees. Possible values are 10–4 ≤≤ angle ≤≤ 360.Note:If pitch >>0, there is no upper limit for angle.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤≤ pitch ≤≤ 105. The default value, 0, implies a normal revolve.

flipRevolveDirection

A Boolean specifying whether to override the direction of feature creation. If *flipRevolveDirection*=OFF, the default direction of revolution is used. If *flipRevolveDirection*=ON, the revolve direction is reversed. The default value is OFF.

flipPitchDirection

A Boolean specifying whether to override the direction of translation. If *flipPitchDirection*=OFF, the direction of translation is given by the direction of the revolve axis. If *flipPitchDirection*=ON, the translation direction is reversed. The default value is OFF.

moveSketchNormalToPath

A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath*=OFF, the sketch plane remains parallel to the revolve axis. If *moveSketchNormalToPath*=ON, the sketch is moved to match the angle created by the *pitch before being revolved. The default value is OFF.

Returns:

A Feature object.

Raises:

RangeError

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseSolidSweep(sketch: ConstrainedSketch, path: ConstrainedSketch)

This method creates a first Feature object by sweeping the given profile ConstrainedSketch object along the path defined by the path ConstrainedSketch object, creating a solid. The profile ConstrainedSketch object must define a closed profile. The origin of the profile sketch is positioned at the start of the sweep path and swept perpendicular to the path. No checks are made for self-intersection.

Parameters:

sketch

A ConstrainedSketch object specifying the profile to be swept.

path

A ConstrainedSketch object specifying the path of the sweep.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BaseWire(sketch: ConstrainedSketch)

This method creates a first Feature object by creating a planar wire from the given ConstrainedSketch object.

Parameters:

sketch

A ConstrainedSketch object specifying the planar wire.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

BlendFaces(side1: tuple[abaqus.BasicGeometry.Edge.Edge], side2: tuple, method: ~abaqusConstants.SymbolicConstantType | None = None, path: ~abaqus.BasicGeometry.Edge.Edge = <abaqus.BasicGeometry.Edge.Edge object>)

This method creates a Feature object by creating new faces that blends two sets of faces.

Parameters:

side1

A sequence of Edge objects specifying one side of the blend. The edges must form a continuous chain without branches.

side2

A sequence of Edge or Face objects specifying the second side of the blend. If side2 contains Edge objects then they must form a continuous chain without branches.

method

A SymbolicConstant indicating a method for creating blends. This argument is a required argument if side2 contains Edge object and it is ignored if side2 contains Faceobjects. It can have one of the following values:TANGENT: The blend is tangent to the sides.SHORTEST_PATH: The blend connects the two sides based on linear interpolation between the two sides.SPECIFY_PATH: The blend connects the two sides along a specified path.

path

An Edge object that connects side1 to side2 and specifies the path for creating the blend. This argument is required if *method*=SPECIFY_PATH; otherwise, it is ignored.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Chamfer(length: float, edgeList: tuple[Edge])

This method creates an additional Feature object by chamfering the given list of edges with a given length.

Parameters:

length

A Float specifying the length of the chamfer.

edgeList

A sequence of Edge objects specifying the edges to chamfer.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

ConvertToAnalytical()

This method attempts to change entities into a simpler form that will speed up processing and make entities available during feature operations.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

ConvertToPrecise(method: SymbolicConstantType = 'RECOMPUTE_GEOMETRY')

This method attempts to change imprecise entities so that the geometry becomes precise.

Parameters:

method

A SymbolicConstant specifying the method to be used to convert the part to precise. Possible values are RECOMPUTE_GEOMETRY and TIGHTEN_GAPS. The default value is RECOMPUTE_GEOMETRY.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

CoverEdges(edgeList: tuple[Edge], tryAnalytical: BooleanType = False)

This method generates a face using the given edges as the face’s boundaries. The CoverEdges method generates a face by creating the geometry consisting of the underlying surface, associated edges, and vertices.

Parameters:

edgeList

A sequence of Edge objects specifying the edges that bound the new face.

tryAnalytical

A Boolean specifying whether the newly created face should be analytical or not. The default is False.

Returns:

A Feature object.

Raises:

• If the given boundary is not a closed loop:

  Parterror: Cannot find a closed loop

• If the given boundary contains a zero length component:

  Parterror: Cannot find a closed loop

• If the underlying surface is too difficult to fit:

  Parterror: Cannot construct face geometry

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Cut(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, sketchOrientation: SymbolicConstantType | None = None)

This method creates an additional Feature object by cutting a hole using the given ConstrainedSketch object.

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketch

A ConstrainedSketch object specifying the planar cut.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

CutExtrude(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketchOrientation: SymbolicConstantType, sketch: ConstrainedSketch, depth: float | None = None, upToFace: str = '', draftAngle: float | None = None, pitch: float | None = None, flipExtrudeDirection: BooleanType = 0)

This method creates an additional Feature object by extruding the given ConstrainedSketch object by the given depth and cutting away material in the solid and shell regions of the part. The ConstrainedSketch object must define a closed profile. The CutExtrude method creates a blind cut (using depth), an up-to-face cut (using upToFace), or a through-all cut (if depth and upToFace are not specified).

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM.

sketch

A ConstrainedSketch object specifying the planar sketch to be extruded.

depth

A Float specifying the extrusion depth. If depth is specified, the cut will be a blind cut. The default is to not specify a depth.

upToFace

A Face specifying the face up to which to cut. If upToFace is specified, the cut will be an up-to-face cut. The default is to not specify a face.Note:If neither depth nor upToFace is specified, the cut will be a through-all cut.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

flipExtrudeDirection

A Boolean specifying whether to override the direction of feature creation. If the value is OFF, it means use the direction defined by the sketchPlaneSide; if the value is ON, it means use the opposite direction to the one defined by sketchPlaneSide. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

CutLoft(loftsections: tuple, startCondition: SymbolicConstantType | None = None, endCondition: SymbolicConstantType | None = None, startTangent: float | None = None, startMagnitude: float | None = None, endTangent: float | None = None, endMagnitude: float | None = None, globalSmoothing: BooleanType = 0)

This method creates an additional Feature object by lofting between the given sections and cutting away material from the part. You define the sections using a sequence of edges from the part or an EdgeArray.

Parameters:

loftsections

A sequence of sequences of edges specifying the cross-sections to be lofted. Each outer sequence specifies a section through which the method will pass the loft feature. Each outer sequence can be defined as a sequence of edges or as an EdgeArray. The edges specifying a section must form a simple closed profile and must not contain multiple loops.

startCondition

A SymbolicConstant specifying the tangent direction at the start section of the loft feature. Possible values are NONE, NORMAL, RADIAL, and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the startCondition argument in conjunction with the endCondition argument.

endCondition

A SymbolicConstant specifying the tangent direction at the end section of the loft feature. Possible values are NONE, NORMAL, RADIAL, and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the endCondition argument in conjunction with the startCondition argument.

startTangent

A Float specifying the angle in degrees of the tangent with respect to the plane in which the start section lies. You must specify the startTangent argument if startCondition*=SPECIFIED. Possible values are 0.0 ≤≤ *startTangent ≤≤ 180.0.

startMagnitude

A Float specifying the magnitude of the startTangent. You must specify the startMagnitude argument if startCondition*=SPECIFIED. Possible values are 0.0 << *startMagnitude << 100.0.

endTangent

A Float specifying the angle in degrees of the tangent with respect to the plane in which the end section lies. You must specify the endTangent argument if startCondition*=SPECIFIED. Possible values are 0.0 ≤≤ *endTangent ≤≤ 180.0.

endMagnitude

A Float specifying the magnitude of the endTangent. This argument is to be used when the endCondition argument has the value SPECIFIED. Possible values are 0.0 << endMagnitude << 100.0.

globalSmoothing

A Boolean specifying whether each path defined in the paths argument is applied locally or globally.If the path is applied locally, its effect is felt only on faces created from the edges on the loftSections through which the paths pass through.If the path is applied globally, an averaging algorithm is applied over all the paths defined and is distributed over all the faces created.The default value is ON (globally).

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

CutRevolve(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketchOrientation: SymbolicConstantType, sketch: ConstrainedSketch, angle: float, pitch: float | None = None, flipRevolveDirection: BooleanType = 0, flipPitchDirection: BooleanType = 0, moveSketchNormalToPath: BooleanType = 0)

This method creates an additional Feature object by revolving the given ConstrainedSketch object by the given angle and cutting away material from the part. The ConstrainedSketch object must define a closed profile and an axis of revolution.

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM.

sketch

A ConstrainedSketch object specifying the planar sketch to be revolved.

angle

A Float specifying the angle in degrees to be revolved.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤≤ pitch ≤≤ 105. The default value, 0, implies a normal revolve.

flipRevolveDirection

A Boolean specifying whether to override the direction of feature creation. If *flipRevolveDirection*=OFF, the default direction of revolution is used. If *flipRevolveDirection*=ON, the revolve direction is reversed. The default value is OFF.

flipPitchDirection

A Boolean specifying whether to override the direction of translation. If *flipPitchDirection*=OFF, the direction of translation is given by the direction of the revolve axis. If *flipPitchDirection*=ON, the translation direction is reversed. The default value is OFF.

moveSketchNormalToPath

A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath*=OFF, the sketch plane remains parallel to the revolve axis. If *moveSketchNormalToPath*=ON, the sketch is moved to match the angle created by the *pitch before being revolved. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

CutSweep(path: str, profile: str, pathPlane: str = '', pathUpEdge: ~abaqus.BasicGeometry.Edge.Edge = <abaqus.BasicGeometry.Edge.Edge object>, pathOrientation: ~abaqusConstants.SymbolicConstantType | None = None, sketchPlane: str = '', sketchUpEdge: ~abaqus.BasicGeometry.Edge.Edge = <abaqus.BasicGeometry.Edge.Edge object>, sketchOrientation: ~abaqusConstants.SymbolicConstantType | None = None, draftAngle: float | None = None, pitch: float | None = None, profileNormal: ~abaqusConstants.BooleanType = 0, flipSweepDirection: ~abaqusConstants.BooleanType = 0)

This method creates an additional Feature object by sweeping the given ConstrainedSketch object along a path which may be a ConstrainedSketch or a sequence of Edge objects and cutting away material from the part. If the profile section is a ConstrainedSketch object, it must define a closed profile. The section sketch can be created at the normal plane at the start of the sweep path or it may be created on a Datum plane or a planar Face. No checks are made for self-intersection.

Parameters:

path

Path may either be a ConstrainedSketch object or a sequence of Edge objects specifying the path of the sweep.

profile

Profile may either be a ConstrainedSketch object or a Face object specifying the section to be swept.

pathPlane

A Datum plane object or a planar Face object. Only required when path is a ConstrainedSketch object.

pathUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the path sketch. Only required when path is a ConstrainedSketch object.

pathOrientation

A SymbolicConstant specifying the orientation of pathUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when path is a ConstrainedSketch object.

sketchPlane

A Datum plane object or a planar Face object specifying the plane on which to sketch the profile. Not required when profile is a Face object. When profile is chosen as a ConstrainedSketch object, user may or may not give this as input. If user does not give this as input, the normal plane at the start of the path will be the sketchPlane.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the profile sketch. Only required when profile is a ConstrainedSketch object.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when profile is a ConstrainedSketch object.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

profileNormal

A Boolean specifying whether to keep the profile normal same as original or varying through out the sweep path. When *profileNormal*=OFF, the profile normal will vary through out the sweep path. When *profileNormal*=ON, the profile normal will be same as original through out the sweep path. The default value is OFF.

flipSweepDirection

A Boolean specifying whether to flip the direction in which sweep operation will be performed. When *flipSweepDirection*=OFF, sweep operation will be performed in the direction of path direction. When *flipSweepDirection*=ON, sweep operation will be performed in the direction opposite to the path direction. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

ExtendFaces(faces: tuple[Face] = (), extendAlong: tuple[Edge] = (), distance: float | None = None, upToFaces: tuple[Face] = (), trimToExtendedTargetSurfaces: BooleanType = True, upToReferenceRep: BooleanType = 0)

This method extends faces along its free edges by offsetting the external edges along the surfaces. One of distance, upToReferenceRep, or upToFaces must be used to specify how far the faces need to be extended.

Parameters:

faces

A sequence of Face objects specifying the faces to be extended. The faces cannot belong to the reference representation. The faces and extendAlong arguments are mutually exclusive. One of them must be specified.

extendAlong

A sequence of Edge objects specifying the edges where to extend the faces. Only free edges are considered. The interior edges will be ignored. The faces and extendAlong arguments are mutually exclusive. One of them must be specified.

distance

A Float indicating the distance to extend the faces along the edges. Either distance, upToReferenceRep, or upToFaces must be specified.

upToFaces

A sequence of Face objects specifying the faces that the selected faces should be extended up to.

trimToExtendedTargetSurfaces

A Boolean indicating that the surfaces of up to target faces should be extended before extending and trimming the selected faces. The default value is True.

upToReferenceRep

A Boolean indicating that the selected faces should be extended along the selected edges and be trimmed along their intersection with the reference representation.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

FaceFromElementFaces(elementFaces: Region, stitch: BooleanType = 0, stitchTolerance: float | None = None, analyticFitTolerance: float | None = None, associateFace: BooleanType = 0)

This method creates a geometry face from a collection of orphan element faces.

Parameters:

elementFaces

A Region object specifying the collection of orphan element faces.

stitch

A Boolean specifying whether the created geometry face should be stitched with existing geometry faces. Default value is TRUE.

stitchTolerance

A Float indicating the maximum gap to be stitched. The value should be smaller than the minimum feature size and bigger than the maximum gap expected to be stitched in the model. Otherwise this command may remove small (sliver) edges that are smaller than the tolerance. If stitch tolerance is not provided then default value of 0.001 will be used for stitching.

analyticFitTolerance

A Float indicating the analytical surface fitting tolerance. If analytical tolerance is not provided then default value of 0.015 will be used for analytical surface fitting.

associateFace

A Boolean specifying whether the created geometry face should be associated with the mesh. Default value is TRUE.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

HoleBlindFromEdges(plane: str, planeSide: SymbolicConstantType, diameter: float, edge1: Edge, distance1: float, edge2: Edge, distance2: float, depth: float)

This method creates an additional Feature object by creating a circular blind hole of the given diameter and depth and cutting away material in the solid and shell regions of the part. The center of the hole is offset from two non-parallel straight edges by the given distances.

Parameters:

plane

A Datum plane object or a planar Face object.

planeSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

diameter

A Float specifying the diameter of the hole.

edge1

An Edge object specifying the edge from which distance1 is measured.

distance1

A Float specifying the offset from edge1.

edge2

An Edge object specifying the edge from which distance2 is measured.

distance2

A Float specifying the offset from edge2.

depth

A Float specifying the depth of the hole.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

HoleFromEdges(diameter: float, edge1: Edge, distance1: float, edge2: Edge, distance2: float)

This method creates an additional Feature object by creating a circular hole of the given diameter in a 2D planar part and cutting away material in the shell and wire regions of the part. The center of the hole is offset from two non-parallel straight edges by the given distances.

Parameters:

diameter

A Float specifying the diameter of the hole.

edge1

An Edge object specifying the edge from which distance1 is measured.

distance1

A Float specifying the offset from edge1.

edge2

An Edge object specifying the edge from which distance2 is measured.

distance2

A Float specifying the offset from edge2.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

HoleThruAllFromEdges(plane: str, planeSide: SymbolicConstantType, diameter: float, edge1: Edge, distance1: float, edge2: Edge, distance2: float)

This method creates an additional Feature object by creating a circular through hole of the given diameter and cutting away material in the solid and shell regions of the part. The center of the hole is offset from two non-parallel straight edges by the given distances.

Parameters:

plane

A Datum plane object or a planar Face object.

planeSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

diameter

A Float specifying the diameter of the hole.

edge1

An Edge object specifying the edge from which distance1 is measured.

distance1

A Float specifying the offset from edge1.

edge2

An Edge object specifying the edge from which distance2 is measured.

distance2

A Float specifying the offset from edge2.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

MergeEdges(edgeList: tuple[Edge] = (), extendSelection: BooleanType = 0)

This method merges edges either by extending the user selection or using only the selected edges.

Parameters:

edgeList

A sequence of Edge objects specifying the edges to be merged.

extendSelection

A Boolean specifying whether the user selection needs to be extended to include edges till branching occurs. Branching is said to occur when the vertex of an edge is shared by more than two edges.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Mirror(mirrorPlane: str, keepOriginal: BooleanType, keepInternalBoundaries: BooleanType = 0)

This method mirrors existing part geometry across a plane to create new geometry.

Parameters:

mirrorPlane

A Datum plane object or a planar Face object.

keepOriginal

A boolean specifying whether or not the original part geometry should be retained.

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

OffsetFaces(faceList: tuple[Face], distance: float | None = None, targetFaces: tuple[Face] = (), targetFacesMethod: SymbolicConstantType | None = None, fractionDistance: float | None = None, trimToReferenceRep: BooleanType = 0)

This method creates new faces by offsetting existing faces.

Parameters:

faceList

A sequence of Face objects specifying the faces that will be offset. The faces may belong to the part or to the reference representation associated with the part.

distance

A Float indicating the distance to offset the faces. Either distance or targetFaces must be specified.

targetFaces

A sequence of Face objects whose distance to the faces argument together with the targetFacesMethod determines the distance to offset the faces. Either distance or targetFaces must be specified.

targetFacesMethod

A SymbolicConstant indicating how to calculate the distance to offset. It can have one of the following values:HALF_OF_AVERAGE: Offset the faces by a distance equals to half the average distance to target faces.CLOSEST_POINT_FRACTION: Offset the faces by a distance equals to the fraction of the distance to the approximate closest point on the selected target faces.FARTHEST_POINT_FRACTION: Offset the faces by a distance equals to the fraction of the distance to the approximate farthest point on the selected target faces.

fractionDistance

A Float indicating the fraction of the distance to the closest or the farthest point on the target faces. Its default value is 0.5.

trimToReferenceRep

A Boolean indicating whether to extend the offset faces and trim them along their intersection with the reference representation.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RemoveCells(cellList: tuple[Cell])

This method converts a solid entity to a shell entity.

Parameters:

cellList

A sequence of Cell objects specifying the cells to remove.

Returns:

A Boolean value.

Raises:

• If the intended volume to be turned into a shell entity is not three-dimensional.

  Parterror: ConstrainedSketchGeometry that is not 3-dimensional does not contain cells.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RemoveFaces(faceList: tuple[Face], deleteCells: BooleanType = False)

This method removes faces from a solid entity or from a shell entity.

Parameters:

faceList

A sequence of Face objects specifying the faces to remove.

deleteCells

A Boolean specifying whether all cells are to be deleted when the faces are removed. The default value is False.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RemoveFacesAndStitch(faceList: tuple[Face])

This method removes faces from a solid entity and attempts to close the resulting gap by extending the neighboring faces of the solid.

Parameters:

faceList

A sequence of Face objects specifying the faces to remove.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RemoveRedundantEntities(vertexList: tuple[Vertex] = (), edgeList: tuple[Edge] = (), removeEdgeVertices: BooleanType = True)

This method removes redundant edges and vertices from a solid or a shell entity. One of the two arguments is required.

Parameters:

vertexList

A sequence of ConstrainedSketchVertex objects specifying the vertices to be removed.

edgeList

A sequence of Edge objects specifying the edges to be removed.

removeEdgeVertices

A Boolean specifying whether the vertices of the redundant edges need to be removed. The default is True.

Returns:

A Feature object.

Raises:

• If the selected entity is not a redundant entity.

  Parterror: None of the selected entities are redundant.

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RepairFaceNormals(faceList: tuple[Face] = ())

This method works on the entire part or a sequence of shell faces. When the entire part is selected, it aligns all the shell face normals, and inverts all of the solid faces’ normals if the solid was originally inside out. When a few shell faces are selected, it inverts the normals of the selected faces.

Parameters:

faceList

A sequence of Face objects.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RepairInvalidEdges(edgeList: tuple[Edge])

This method repairs invalid edges. It will always attempt to improve edges even if none of selected edges are initially invalid and may leave behind invalid edges that could not be repaired.

Parameters:

edgeList

A sequence of Edge objects.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RepairSliver(face: Face, point1: int, point2: int, toleranceChecks: BooleanType = True)

This method repairs the selected sliver from the selected face. The sliver area is specified using two points. A face partition is carried out at the specified points and the smaller of the two faces is removed.

Parameters:

face

A Face object specifying the face on which the sliver is located.

point1

A point specifying the location for partition creation. It can be a ConstrainedSketchVertex object, an Interesting Point or three coordinates specifying the point on an edge of the face.

point2

A point specifying the location for partition creation. It can be a ConstrainedSketchVertex object, an Interesting Point or three coordinates specifying the point on an edge of the face.

toleranceChecks

A Boolean specifying whether to use internal tolerance checks to restrict the size of the sliver face being removed. The default is True.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RepairSmallEdges(edgeList: tuple[Edge], toleranceChecks: BooleanType = True)

This method repairs small edges. This method will attempt to replace selected small edges with vertices and extend the adjacent faces and edges. This method might leave behind some small edges that cannot be removed.

Parameters:

edgeList

A sequence of Edge objects.

toleranceChecks

A Boolean specifying whether to use internal tolerance checks to restrict the size of the edges being removed. The default is True.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

RepairSmallFaces(faceList: tuple[Face], toleranceChecks: BooleanType = True)

This method repairs small faces. It will attempt to replace the selected small faces with edges or vertices and extend the adjacent faces. This method might leave behind some small faces that cannot be removed.

Parameters:

faceList

A sequence of Face objects.

toleranceChecks

A Boolean specifying whether to use internal tolerance checks to restrict the size of the faces being removed. The default is True.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

ReplaceFaces(faceList: tuple[Face], stitch: BooleanType = True)

This method replaces the selected faces with a single face. If one single face is selected, that alone is replaced with a new face.

Parameters:

faceList

A sequence of Face objects to be replaced.

stitch

A Boolean specifying whether the newly created face needs to be stitched to the existing geometry. The default is True.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Round(radius: float, edgeList: tuple[Edge], vertexList: tuple[Vertex])

This method creates an additional Feature object by rounding (filleting) the given list of entities with the given radius.

Parameters:

radius

A Float specifying the radius of the fillets.

edgeList

A sequence of Edge objects. Solid and Shell edges of a part can be rounded. The operation will fail for non-manifold edges. The edgeList and vertexList arguments are mutually exclusive. One of them must be specified.

vertexList

A sequence of ConstrainedSketchVertex objects. Vertices that are connected to two wire edges can be rounded. The operation will fail for a vertex connected to a face. The edgeList and vertexList arguments are mutually exclusive. One of them must be specified.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Shell(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, sketchOrientation: SymbolicConstantType = 'RIGHT')

This method creates an additional Feature object by creating a planar shell from the given ConstrainedSketch object. The ConstrainedSketch object must define a closed profile.

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketch

A ConstrainedSketch object specifying the planar shell.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

ShellExtrude(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, depth: float | None = None, upToFace: str = '', sketchOrientation: SymbolicConstantType = 'RIGHT', draftAngle: float | None = None, pitch: float | None = None, flipExtrudeDirection: BooleanType = 0, keepInternalBoundaries: BooleanType = 0)

This method creates an additional Feature object by extruding the given ConstrainedSketch object by the given depth, creating a shell protrusion. The ConstrainedSketch object can define either an open or closed profile.

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketch

A ConstrainedSketch object specifying the planar sketch to be extruded.

depth

A Float specifying the extrusion depth. The default is to not specify a depth. Either depth or upToFace must be used to define the extrusion depth.

upToFace

A Face specifying the face up to which to extrude. If upToFace is specified, the extrusion will be an up-to-face extrusion. The default is to not specify a face. Either depth or upToFace must be used to define the extrusion depth.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

flipExtrudeDirection

A Boolean specifying whether to override the direction of feature creation. If the value is OFF, it means use the direction defined by the sketchPlaneSide; if the value is ON, it means use the opposite direction to the one defined by sketchPlaneSide. The default value is OFF.

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

ShellLoft(loftsections: tuple, startCondition: SymbolicConstantType | None = None, endCondition: SymbolicConstantType | None = None, startTangent: float | None = None, startMagnitude: float | None = None, endTangent: float | None = None, endMagnitude: float | None = None, paths: tuple = (), globalSmoothing: BooleanType = 0, keepInternalBoundaries: BooleanType = 0)

This method creates an additional Feature object by lofting between the given sections and adding shell faces to the part. You define the sections using a sequence of edges from the part or an EdgeArray.

Parameters:

loftsections

A sequence of sequences of edges specifying the cross-sections to be lofted. Each outer sequence specifies a section through which the method will pass the loft feature. Each outer sequence can be defined as a sequence of edges or as an EdgeArray. The edges specifying a section must form a simple closed profile and must not contain multiple loops.

startCondition

A SymbolicConstant specifying the tangent direction at the start section of the loft feature. Possible values are NONE, NORMAL, RADIAL and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the startCondition argument in conjunction with the endCondition argument.

endCondition

A SymbolicConstant specifying the tangent direction at the end section of the loft feature. Possible values are NONE, NORMAL, RADIAL and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the endCondition argument in conjunction with the startCondition argument.

startTangent

A Float specifying the angle in degrees of the tangent with respect to the plane in which the start section lies. You must specify the startTangent argument if startCondition*=SPECIFIED. Possible values are 0.0 ≤≤ *startTangent ≤≤ 180.0.

startMagnitude

A Float specifying the magnitude of the startTangent. You must specify the startMagnitude argument if startCondition*=SPECIFIED. Possible values are 0.0 << *startMagnitude << 100.0.

endTangent

A Float specifying the angle in degrees of the tangent with respect to the plane in which the end section lies. You must specify the endTangent argument if startCondition*=SPECIFIED. Possible values are 0.0 ≤≤ *endTangent ≤≤ 180.0.

endMagnitude

A Float specifying the magnitude of the endTangent. This argument is to be used when the endCondition argument has the value SPECIFIED. Possible values are 0.0 << endMagnitude << 100.0.

paths

A sequence of sequences of edges that pass through each section in the loft feature. Each sequence specifies a path followed by the face or an edge created by a loft feature. Each path must start at the first section, end at the last section, and pass through each section. In addition, the order of the sequences must be the same as the order of the sections in the loftsections argument. Each path must not self-intersect and must be tangent continuous. In addition, the paths must not intersect each other. You cannot use the paths argument in conjunction with the startCondition and endCondition arguments.

globalSmoothing

A Boolean specifying whether each path defined in the paths argument is applied locally or globally.If the path is applied locally, its effect is felt only on faces created from the edges on the loftsections through which the paths pass through.If the path is applied globally, an averaging algorithm is applied over all the paths defined and is distributed over all the faces created.The default value is ON (globally).

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

ShellRevolve(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, angle: float, sketchOrientation: SymbolicConstantType = 'RIGHT', pitch: float | None = None, flipRevolveDirection: BooleanType = 0, flipPitchDirection: BooleanType = 0, moveSketchNormalToPath: BooleanType = 0, keepInternalBoundaries: BooleanType = 0)

This method creates an additional Feature object by revolving the given ConstrainedSketch object by the given angle, creating a shell protrusion. The ConstrainedSketch object can define either an open or closed profile and an axis of revolution. The axis is defined by a single construction line. For a description of the plane positioning arguments, see SolidExtrude.

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketch

A ConstrainedSketch object specifying the planar sketch to be revolved.

angle

A Float specifying the angle in degrees to be revolved.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤≤ pitch ≤≤ 105. The default value, 0, implies a normal revolve.

flipRevolveDirection

A Boolean specifying whether to override the direction of feature creation. If *flipRevolveDirection*=OFF, the default direction of revolution is used. If *flipRevolveDirection*=ON, the revolve direction is reversed. The default value is OFF.

flipPitchDirection

A Boolean specifying whether to override the direction of translation. If *flipPitchDirection*=OFF, the direction of translation is given by the direction of the revolve axis. If *flipPitchDirection*=ON, the translation direction is reversed. The default value is OFF.

moveSketchNormalToPath

A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath*=OFF, the sketch plane remains parallel to the revolve axis. If *moveSketchNormalToPath*=ON, the sketch is moved to match the angle created by the *pitch before being revolved. The default value is OFF.

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

ShellSweep(path: str, profile: str, pathPlane: str = '', pathUpEdge: ~abaqus.BasicGeometry.Edge.Edge = <abaqus.BasicGeometry.Edge.Edge object>, pathOrientation: ~abaqusConstants.SymbolicConstantType | None = None, sketchPlane: str = '', sketchUpEdge: ~abaqus.BasicGeometry.Edge.Edge = <abaqus.BasicGeometry.Edge.Edge object>, sketchOrientation: ~abaqusConstants.SymbolicConstantType | None = None, draftAngle: float | None = None, pitch: float | None = None, profileNormal: ~abaqusConstants.BooleanType = 0, flipSweepDirection: ~abaqusConstants.BooleanType = 0, keepInternalBoundaries: ~abaqusConstants.BooleanType = 0)

This method creates an additional Feature object by sweeping the given ConstrainedSketch object or a sequence of Edge objects along a path which may be a ConstrainedSketch or a sequence of Edge objects, creating a shell swept protrusion. The section can be an open or a closed profile. The section sketch can be created at the normal plane at the start of the sweep path or it may be created on a Datum plane or a planar Face. No checks are made for self-intersection.

Parameters:

path

Path may either be a ConstrainedSketch object or a sequence of Edge objects specifying the path of the sweep.

profile

Profile may either be a ConstrainedSketch object or a sequence of Edge objects specifying the section to be swept.

pathPlane

A Datum plane object or a planar Face object. Only required when path is a ConstrainedSketch object.

pathUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the path sketch. Only required when path is a ConstrainedSketch object.

pathOrientation

A SymbolicConstant specifying the orientation of pathUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when path is a ConstrainedSketch object.

sketchPlane

A Datum plane object or a planar Face object specifying the plane on which to sketch the profile. Not required when profile is a Face object. When profile is chosen as ConstrainedSketch object, user may or may not give this as input. If user does not give this as input, the normal plane at the start of the path will be the sketchPlane.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the profile sketch. Only required when profile is a ConstrainedSketch object.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when profile is a ConstrainedSketch object.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

profileNormal

A Boolean specifying whether to keep the profile normal same as original or varying through out the sweep path. When *profileNormal*=OFF, the profile normal will vary through out the sweep path. When *profileNormal*=ON, the profile normal will be same as original through out the sweep path. The default value is OFF.

flipSweepDirection

A Boolean specifying whether to flip the direction in which sweep operation will be performed. When *flipSweepDirection*=OFF, sweep operation will be performed in the direction of path direction. When *flipSweepDirection*=ON, sweep operation will be performed in the direction opposite to the path direction. The default value is OFF.

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

SolidExtrude(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, depth: float | None = None, upToFace: str = '', sketchOrientation: SymbolicConstantType = 'RIGHT', draftAngle: float | None = None, pitch: float | None = None, flipExtrudeDirection: BooleanType = 0, keepInternalBoundaries: BooleanType = 0)

This method creates an additional Feature object by extruding the given ConstrainedSketch object by the given depth, creating a solid protrusion. The ConstrainedSketch object must define a closed profile.

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketch

A ConstrainedSketch object specifying the planar sketch to be extruded.

depth

A Float specifying the extrusion depth. The default is to not specify a depth. Either depth or upToFace must be used to define the extrusion depth.

upToFace

A Face specifying the face up to which to extrude. If upToFace is specified, the extrusion will be an up-to-face extrusion. The default is to not specify a face. Either depth or upToFace must be used to define the extrusion depth.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

flipExtrudeDirection

A Boolean specifying whether to override the direction of feature creation. If the value is OFF, it means use the direction defined by the sketchPlaneSide; if the value is ON, it means use the opposite direction to the one defined by sketchPlaneSide. The default value is OFF.

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

SolidLoft(loftsections: tuple, startCondition: SymbolicConstantType | None = None, endCondition: SymbolicConstantType | None = None, startTangent: float | None = None, startMagnitude: float | None = None, endTangent: float | None = None, endMagnitude: float | None = None, paths: tuple = (), globalSmoothing: BooleanType = 0, keepInternalBoundaries: BooleanType = 0)

This method creates an additional Feature object by lofting between the given sections and adding material to the part. You define the sections using a sequence of edges from the part or an EdgeArray.

Parameters:

loftsections

A sequence of sequences of edges specifying the cross-sections to be lofted. Each outer sequence specifies a section through which Abaqus will pass the loft feature. Each outer sequence can be defined as a sequence of edges or as an EdgeArray. The edges specifying a section must form a simple closed profile and must not contain multiple loops.

startCondition

A SymbolicConstant specifying the tangent direction at the start section of the loft feature. Possible values are NONE, NORMAL, RADIAL and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the startCondition argument in conjunction with the endCondition argument.

endCondition

A SymbolicConstant specifying the tangent direction at the end section of the loft feature. Possible values are NONE, NORMAL, RADIAL and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the endCondition argument in conjunction with the startCondition argument.

startTangent

A Float specifying the angle in degrees of the tangent with respect to the plane in which the start section lies. You must specify the startTangent argument if startCondition*=SPECIFIED. Possible values are 0.0 ≤≤ *startTangent ≤≤ 180.0.

startMagnitude

A Float specifying the magnitude of the startTangent. You must specify the startMagnitude argument if startCondition*=SPECIFIED. Possible values are 0.0 << *startMagnitude << 100.0.

endTangent

A Float specifying the angle in degrees of the tangent with respect to the plane in which the end section lies. You must specify the endTangent argument if startCondition*=SPECIFIED. Possible values are 0.0 ≤≤ *endTangent ≤≤ 180.0.

endMagnitude

A Float specifying the magnitude of the endTangent. This argument is to be used when the endCondition argument has the value SPECIFIED. Possible values are 0.0 << endMagnitude << 100.0.

paths

A sequence of sequences of edges that pass through each section in the loft feature. Each sequence specifies a path followed by the face or an edge created by a loft feature. Each path must start at the first section, end at the last section, and pass through each section. In addition, the order of the sequences must be the same as the order of the sections in the loftsections argument. Each path must not self-intersect and must be tangent continuous. In addition, the paths must not intersect each other. You cannot use the paths argument in conjunction with the startCondition and endCondition arguments.

globalSmoothing

A Boolean specifying whether each path defined in the paths argument is applied locally or globally.If the path is applied locally, its effect is felt only on faces created from the edges on the loftsections through which the paths pass through.If the path is applied globally, an averaging algorithm is applied over all the paths defined and is distributed over all the faces created.The default value is ON (globally).

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

SolidRevolve(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, angle: float, sketchOrientation: SymbolicConstantType = 'RIGHT', pitch: float | None = None, flipRevolveDirection: BooleanType = 0, flipPitchDirection: BooleanType = 0, moveSketchNormalToPath: BooleanType = 0, keepInternalBoundaries: BooleanType = 0)

This method creates an additional Feature object by revolving the given ConstrainedSketch object by the given angle, creating a solid protrusion. The ConstrainedSketch object must define a closed profile and an axis of revolution. The axis is defined by a single construction line.

Parameters:

sketchPlane

A Datum plane object or a planar Face object.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketch

A ConstrainedSketch object specifying the planar sketch to be revolved.

angle

A Float specifying the angle in degrees to be revolved.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤≤ pitch ≤≤ 105. The default value, 0, implies a normal revolve.

flipRevolveDirection

A Boolean specifying whether to override the direction of feature creation. If *flipRevolveDirection*=OFF, the default direction of revolution is used. If *flipRevolveDirection*=ON, the revolve direction is reversed. The default value is OFF.

flipPitchDirection

A Boolean specifying whether to override the direction of translation. If *flipPitchDirection*=OFF, the direction of translation is given by the direction of the revolve axis. If *flipPitchDirection*=ON, the translation direction is reversed. The default value is OFF.

moveSketchNormalToPath

A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath*=OFF, the sketch plane remains parallel to the revolve axis. If *moveSketchNormalToPath*=ON, the sketch is moved to match the angle created by the *pitch before being revolved. The default value is OFF.

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

SolidSweep(path: str, profile: str, pathPlane: str = '', pathUpEdge: ~abaqus.BasicGeometry.Edge.Edge = <abaqus.BasicGeometry.Edge.Edge object>, pathOrientation: ~abaqusConstants.SymbolicConstantType | None = None, sketchPlane: str = '', sketchUpEdge: ~abaqus.BasicGeometry.Edge.Edge = <abaqus.BasicGeometry.Edge.Edge object>, sketchOrientation: ~abaqusConstants.SymbolicConstantType | None = None, draftAngle: float | None = None, pitch: float | None = None, profileNormal: ~abaqusConstants.BooleanType = 0, flipSweepDirection: ~abaqusConstants.BooleanType = 0, keepInternalBoundaries: ~abaqusConstants.BooleanType = 0)

This method creates an additional Feature object by sweeping the given ConstrainedSketch object or a Face object along a path which may be a ConstrainedSketch or a sequence of Edge objects, creating a solid swept protrusion. If the profile section is a ConstrainedSketch object, it must define a closed profile. The section sketch can be created at the normal plane at the start of the sweep path or it may be created on a Datum plane or a planar Face. No checks are made for self-intersection.

Parameters:

path

Path may either be a ConstrainedSketch object or a sequence of Edge objects specifying the path of the sweep.

profile

Profile may either be a ConstrainedSketch object or a Face object specifying the section to be swept.

pathPlane

A Datum plane object or a planar Face object. Only required when path is a ConstrainedSketch object.

pathUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the path sketch. Only required when path is a ConstrainedSketch object.

pathOrientation

A SymbolicConstant specifying the orientation of pathUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when path is a ConstrainedSketch object.

sketchPlane

A Datum plane object or a planar Face object specifying the plane on which to sketch the profile. Not required when profile is a Face object. When profile is chosen as ConstrainedSketch object, user may or may not give this as input. If user does not give this as input, the normal plane at the start of the path will be the sketchPlane.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the profile sketch. Only required when profile is a ConstrainedSketch object.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when profile is a ConstrainedSketch object.

draftAngle

A Float specifying the draft angle in degrees. Possible values are -90.0 ≤≤ draftAngle ≤≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.

pitch

A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are –105 ≤≤ pitch ≤≤ 105. The arguments draftAngle and pitch are mutually exclusive.

profileNormal

A Boolean specifying whether to keep the profile normal same as original or varying through out the sweep path. When *profileNormal*=OFF, the profile normal will vary through out the sweep path. When *profileNormal*=ON, the profile normal will be same as original through out the sweep path. The default value is OFF.

flipSweepDirection

A Boolean specifying whether to flip the direction in which sweep operation will be performed. When *flipSweepDirection*=OFF, sweep operation will be performed in the direction of path direction. When *flipSweepDirection*=ON, sweep operation will be performed in the direction opposite to the path direction. The default value is OFF.

keepInternalBoundaries

A Boolean specifying whether internal boundaries will be retained. The default value is OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Stitch(edgeList: tuple[Edge] = (), stitchTolerance: float | None = None)

This method attempts to create a valid part by binding together free and imprecise edges of all the faces of a part. If edgeList is not given, a global stitch will be performed. If stitchTolerance is not specified, a value of 1.0 will be used.

Parameters:

edgeList

A sequence of Edge objects specifying the edges that need to be stitched.

stitchTolerance

A Float indicating the maximum gap to be stitched. The value should be smaller than the minimum feature size and bigger than the maximum gap expected to be stitched in the model. Otherwise this command may remove small (sliver) edges that are smaller than the tolerance.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

Wire(sketchPlane: str, sketchPlaneSide: SymbolicConstantType, sketchUpEdge: Edge, sketch: ConstrainedSketch, sketchOrientation: SymbolicConstantType = 'RIGHT')

This method creates an additional Feature object by creating a planar wire from the given ConstrainedSketch object. The ConstrainedSketch object must define a closed profile.

Parameters:

sketchPlane

A Datum plane object or a planar Face object specifying the plane on which to sketch.

sketchPlaneSide

A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.

sketchUpEdge

An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.

sketch

A ConstrainedSketch object specifying the planar sketch to be revolved.

sketchOrientation

A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

WireFromEdge(edgeList: str)

This method creates an additional Feature object by creating a Wire by selecting one or more Edge objects of a Solid or Shell part.

Parameters:

edgeList

A list of Edge objects specifying the edges from which the wire is to be created.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

WirePolyLine(points: tuple, mergeType: SymbolicConstantType = 'IMPRINT', meshable: BooleanType = 1)

This method creates an additional Feature object by creating a polyline wire that passes through a sequence of given points. Each point can be a datum point, a vertex, an interesting point, or a tuple.

Parameters:

points

A sequence of ConstrainedSketchVertex, Datum point, or InterestingPoint objects specifying the points through which the polyline wire will pass. points can also be a sequence of tuples of Floats. You must specify at least two values in the sequence.

mergeType

A SymbolicConstant specifying the merge behavior of the wire with existing geometry. If mergeType is MERGE, Abaqus merges the wire into solid regions of the part if the wire passes through them. If mergeType is IMPRINT, Abaqus imprints the wire on existing geometry as edges. If mergeType is SEPARATE, Abaqus neither merges nor imprints the spline wire with existing geometry. It creates the wire separately. The default value is IMPRINT.

meshable

A Boolean specifying whether the wire should be available for selection in meshing operations. If *meshable*=OFF, the wire can be used for connector section assignment. The default value is ON.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair

WireSpline(points: tuple, mergeType: SymbolicConstantType = 'IMPRINT', smoothClosedSpline: BooleanType = 0)

This method creates an additional Feature object by creating a spline wire that passes through a sequence of given points. Each point can be a datum point, a vertex, an interesting point, or a tuple.

Parameters:

points

A sequence of ConstrainedSketchVertex, Datum point, or InterestingPoint objects specifying the points through which the spline wire will pass. points can also be a sequence of tuples of Floats. You must specify at least two values in the sequence.

mergeType

A SymbolicConstant specifying the merge behavior of the wire with existing geometry. If mergeType is MERGE, Abaqus merges the wire into solid regions of the part if the wire passes through them. If mergeType is IMPRINT, Abaqus imprints the spline wire on existing geometry as edges. If mergeType is SEPARATE, Abaqus neither merges nor imprints the spline wire with existing geometry. It creates the wire separately. The default value is IMPRINT.

smoothClosedSpline

A Boolean specifying the behavior of Abaqus when the points defining a spline wire form a closed loop (the start and end points are the same). If *smoothClosedSpline*=ON, Abaqus creates a smooth spline wire where the tangencies at the end point meet smoothly. If *smoothClosedSpline*=OFF, Abaqus does not automatically create a smooth end condition. The default value in OFF.

Returns:

feature: Feature

A Feature object

Notes

This function can be accessed by:

mdb.models[name].parts[*name*].AutoRepair