Mesh

Mesh commands are used to mesh part instances and regions. Mesh commands are also used to assign element sizes, element types, and mesh control parameters.

Object features

Mesh features for Assembly

class MeshAssembly

An Assembly object is a container for instances of parts. The Assembly object has no constructor command. Abaqus creates the rootAssembly member when a Model object is created.

Note

This object can be accessed by:

import assembly
mdb.models[name].rootAssembly

Note

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

Public Data Attributes:

Inherited from AssemblyBase

isOutOfDate	An Int specifying that feature parameters have been modified but that the assembly has not been regenerated.
timeStamp	A Float specifying which gives an indication when the assembly was last modified.
isLocked	An Int specifying whether the assembly is locked or not.
regenerateConstraintsTogether	A Boolean specifying whether the positioning constraints in the assembly should be regenerated together before regenerating other assembly features.
vertices	A VertexArray object specifying all the vertices existing at the assembly level.
edges	An EdgeArray object specifying all the edges existing at the assembly level.
elements	A MeshElementArray object specifying all the elements existing at the assembly level.
nodes	A MeshNodeArray object specifying all the nodes existing at the assembly level.
instances	A repository of PartInstance objects.
datums	A repository of Datum objects specifying all Datum objects in the assembly.
features	A repository of Feature objects specifying all Feature objects in the assembly.
featuresById	A repository of Feature objects specifying all Feature objects in the assembly.The Feature objects in the featuresById repository are the same as the Feature objects in the features repository.
surfaces	A repository of Surface objects specifying for more information, see [Region commands](https://help.3ds.com/2022/english/DSSIMULIA_Established/SIMACAEKERRefMap/simaker-m-RegPyc-sb.htm?ContextScope=all).
allSurfaces	A repository of Surface objects specifying for more information, see [Region commands](https://help.3ds.com/2022/english/DSSIMULIA_Established/SIMACAEKERRefMap/simaker-m-RegPyc-sb.htm?ContextScope=all).
allInternalSurfaces	A repository of Surface objects specifying picked regions.
sets	A repository of Set objects.
allSets	A repository of Set objects specifying for more information, see [Region commands](https://help.3ds.com/2022/english/DSSIMULIA_Established/SIMACAEKERRefMap/simaker-m-RegPyc-sb.htm?ContextScope=all).
allInternalSets	A repository of Set objects specifying picked regions.
skins	A repository of Skin objects specifying the skins created on the assembly.
stringers	A repository of Stringer objects specifying the stringers created on the assembly.
referencePoints	A repository of ReferencePoint objects.
modelInstances	A repository of ModelInstance objects.
allInstances	A PartInstance object specifying the PartInstances and A ModelInstance object specifying the ModelInstances.
engineeringFeatures	An EngineeringFeature object.
modelName	A String specifying the name of the model to which the assembly belongs.
connectorOrientations	A ConnectorOrientationArray object.
sectionAssignments	A SectionAssignmentArray object.

Inherited from Feature

name	A String specifying the repository key.
id	An Int specifying the ID of the feature.

Public Methods:

assignStackDirection(cells, referenceRegion)	This method assigns a stack direction to geometric cells.
associateMeshWithGeometry(geometricEntity[, ...])	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.
createVirtualTopology(regions[, ...])	This method creates a virtual topology feature by automatically merging faces and edges based on a set of geometric parameters.
deleteBoundaryLayerControls(regions)	This method deletes the control parameters for boundary layer mesh for all the specified regions.
deleteMesh(regions)	This method deletes a subset of the mesh that contains the native elements from the given part instances or regions.
deleteMeshAssociationWithGeometry(...[, ...])	This method deletes the association of geometric entities with mesh entities.
deletePreviewMesh()	This method deletes all boundary meshes in the assembly.
deleteSeeds(regions)	This method deletes the global edge seeds from the given part instances or deletes the local edge seeds from the given edges.
generateBottomUpExtrudedMesh(cell, ...[, ...])	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.
generateBottomUpSweptMesh(cell[, ...])	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.
generateBottomUpRevolvedMesh(cell, ...[, ...])	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.
generateMesh([regions, ...])	This method generates a mesh in the given part instances or regions.
getEdgeSeeds(edge, attribute)	This method returns an edge seed parameter for a specified edge of an assembly.
getElementType(region, elemShape)	This method returns the ElemType object of a given element shape assigned to a region of the assembly.
getIncompatibleMeshInterfaces([cells])	This method returns a sequence of face objects that are meshed with incompatible elements.
getMeshControl(region, attribute)	This method returns a mesh control parameter for the specified region of the assembly.
getMeshStats(regions)	This method returns the mesh statistics for the given part instances or regions.
getPartSeeds(region, attribute)	This method returns a part seed parameter for the specified instance.
getUnmeshedRegions()	This method returns all geometric regions in the assembly that require a mesh for submitting an analysis but are either unmeshed or are meshed incompletely.
ignoreEntity(entities)	This method creates a virtual topology feature.
restoreIgnoredEntity(entities)	This method restores vertices and edges that have been merged using a virtual topology feature.
seedEdgeByBias(biasMethod, end1Edges, ...[, ...])	This method seeds the given edges nonuniformly using the specified number of elements and bias ratio or the specified minimum and maximum element sizes.
seedEdgeByNumber(edges, number[, constraint])	This method seeds the given edges uniformly based on the number of elements along the edges.
seedEdgeBySize(edges, size[, ...])	This method seeds the given edges either uniformly or following edge curvature distribution, based on the desired element size.
seedPartInstance(regions, size[, ...])	This method assigns global edge seeds to the given part instances.
setBoundaryLayerControls(regions, ...[, ...])	This method sets the control parameters for boundary layer mesh for the specified regions.
setElementType(regions, elemTypes)	This method assigns element types to the specified regions.
setLogicalCorners(region, corners)	This method sets the logical corners for a mappable face region.
setMeshControls(regions[, elemShape, ...])	This method sets the mesh control parameters for the specified regions.
setSweepPath(region, edge, sense)	This method sets the sweep path for a sweepable region or the revolve path for a revolvable region.
verifyMeshQuality(criterion[, threshold, ...])	This method tests the quality of part instance meshes and returns poor-quality elements.

Inherited from AssemblyBase

Instance(name, *args, **kwargs)	This method creates a PartInstance object and puts it into the instances repository.
backup()	This method makes a backup copy of the features in the assembly.
clearGeometryCache()	This method deletes the geometry cache.
deleteAllFeatures()	This method deletes all the features in the assembly.
deleteFeatures(featureNames)	This method deletes specified features from the assembly.
excludeFromSimulation(instances, exclude)	This method excludes the specified part instances from the analysis.
featurelistInfo()	This method prints the name and status of all the features in the feature lists.
getMassProperties([regions, ...])	This method returns the mass properties of the assembly, or instances or regions.
getAngle(plane1, plane2, line1, line2[, ...])	This method returns the angle between the specified entities.
getCoordinates(entity)	This method returns the coordinates of a specified point.
getDistance(entity1, entity2[, ...])	Depending on the arguments provided, this method returns one of the following:
getFacesAndVerticesOfAttachmentLines(edges)	Given an array of edge objects, this method returns a tuple of dictionary objects.
getSurfaceSections(surface)	This method returns a list of the sections assigned to the regions encompassed by the specified surface.
importEafFile(filename[, ids])	This method imports an assembly from an EAF file into the root assembly.
importParasolidFile(filename[, ids])	This method imports an assembly from the Parasolid file into the root assembly.
importCatiaV5File(filename[, ids])	This method imports an assembly from a CATIA V5 Elysium Neutral file into the root assembly.
importEnfFile(filename[, ids])	This method imports an assembly from an Elysium Neutral file created by Pro/ENGINEER, I-DEAS, or CATIA V5 into the root assembly.
importIdeasFile(filename[, ids])	This method imports an assembly from an I-DEAS Elysium Neutral file into the root assembly.
importProEFile(filename[, ids])	This method imports an assembly from a Pro/ENGINEER Elysium Neutral file into the root assembly.
makeDependent(instances)	This method converts the specified part instances from independent to dependent part instances.
makeIndependent(instances)	This method converts the specified part instances from dependent to independent part instances.
printAssignedSections()	This method prints a summary of assigned connector sections.
printConnectorOrientations()	This method prints a summary of connector orientations.
projectReferencesOntoSketch(sketch[, ...])	This method projects the specified edges, vertices, and datum points from the assembly onto the specified ConstrainedSketch object.
queryCachedStates()	This method displays the position of geometric states relative to the sequence of features in the assembly cache.
regenerate()	This method regenerates the assembly and brings it up to date with the latest values of the assembly parameters.
regenerationWarnings()	This method prints any regeneration warnings associated with the features.
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 or assembly.
resumeFeatures(featureNames)	This method resumes the specified suppressed features in the assembly.
resumeLastSetFeatures()	This method resumes the last set of features to be suppressed in the assembly.
rotate(instanceList, axisPoint, ...)	This method rotates given instances by the specified amount.
translate(instanceList, vector)	This method translates given instances by the specified amount.
saveGeometryCache()	This method caches the current geometry, which improves regeneration performance.
setValues(regenerateConstraintsTogether)	This method modifies the behavior associated with the specified assembly.
suppressFeatures(featureNames)	This method suppresses specified features.
unlinkInstances(instances)	This method converts the specified PartInstance objects from linked child instances to regular instances.
writeAcisFile(fileName[, version])	This method exports the assembly to a named file in ACIS part (SAT) or assembly (ASAT) format.
writeCADParameters(paramFile[, ...])	This method writes the parameters that were imported from the CAD system to a parameter file.
lock()	This method locks the assembly.
unlock()	This method unlocks the assembly.
setMeshNumberingControl(instances[, ...])	This method changes the start node and/or element labels on the specified independent part instances before or after Abaqus/CAE generates the meshes.
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.
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

Inherited from AssemblyFeature

AttachmentLines(name, points, sourceFaces, ...)	This method creates a Feature object by creating attachment lines between the given set of source and target faces.
Coaxial(movableAxis, fixedAxis, flip)	This method moves an instance so that its selected face is coaxial with the selected face of a fixed instance.
CoincidentPoint(movablePoint, fixedPoint)	This method moves an instance so that a specified point is coincident with a specified point of a fixed instance.
EdgeToEdge(movableAxis, fixedAxis, flip, ...)	This method moves an instance so that its edge is parallel to an edge of a fixed instance.
FaceToFace(movablePlane, fixedPlane, flip, ...)	This method moves an instance so that its face is coincident with a face of a fixed instance.
ParallelCsys(movableCsys, fixedCsys)	This method moves an instance so that its Datum coordinate system is parallel to a Datum coordinate system of a fixed instance.
ParallelEdge(movableAxis, fixedAxis, flip)	This method moves an instance so that its edge is parallel to an edge of a fixed instance.
ParallelFace(movablePlane, fixedPlane, flip)	This method moves an instance so that its face is parallel to a face of a fixed instance.

Inherited from Feature

AttachmentPoints(name, points[, ...])	This method creates an attachment points Feature.
AttachmentPointsAlongDirection(name, ...[, ...])	This method creates a Feature object by creating attachment points along a direction or between two points.
AttachmentPointsOffsetFromEdges(name, edges)	This method creates a Feature object by creating attachment points along or offset from one or more connected edges.
DatumAxisByCylFace(face)	This method creates a Feature object and a DatumAxis object along the axis of a cylinder or cone.
DatumAxisByNormalToPlane(plane, point)	This method creates a Feature object and a DatumAxis object normal to the specified plane and passing through the specified point.
DatumAxisByParToEdge(edge, point)	This method creates a Feature object and a DatumAxis object parallel to the specified edge and passing through the specified point.
DatumAxisByPrincipalAxis(principalAxis)	This method creates a Feature object and a DatumAxis object along one of the three principal axes.
DatumAxisByRotation(*args, **kwargs)
DatumAxisByThreePoint(point1, point2, point3)	This method creates a Feature object and a DatumAxis object normal to the circle described by three points and through its center.
DatumAxisByThruEdge(edge)	This method creates a Feature object and a DatumAxis object along the specified edge.
DatumAxisByTwoPlane(plane1, plane2)	This method creates a Feature object and a DatumAxis object at the intersection of two planes.
DatumAxisByTwoPoint(point1, point2)	This method creates a Feature object and a DatumAxis object along the line joining two points.
DatumCsysByDefault(coordSysType[, name])	This method creates a Feature object and a DatumCsys object from the specified default coordinate system at the origin.
DatumCsysByOffset(coordSysType, ...[, name])	This method creates a Feature object and a DatumCsys object by offsetting the origin of an existing datum coordinate system to a specified point.
DatumCsysByThreePoints(coordSysType, origin, ...)	This method creates a Feature object and a DatumCsys object from three points.
DatumCsysByTwoLines(coordSysType, line1, line2)	This method creates a Feature object and a DatumCsys object from two orthogonal lines.
DatumPlaneByPrincipalPlane(principalPlane, ...)	This method creates a Feature object and a DatumPlane object through the origin along one of the three principal planes.
DatumPlaneByOffset(*args, **kwargs)
DatumPlaneByRotation(plane, axis, angle)	This method creates a Feature object and a DatumPlane object by rotating a plane about the specified axis through the specified angle.
DatumPlaneByThreePoints(point1, point2, point3)	This method creates a Feature object and a DatumPlane object defined by passing through three points.
DatumPlaneByLinePoint(line, point)	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.
DatumPlaneByPointNormal(point, normal)	This method creates a Feature object and a DatumPlane object normal to the specified line and running through the specified point.
DatumPlaneByTwoPoint(point1, point2)	This method creates a Feature object and a DatumPlane object midway between two points and normal to the line connecting the points.
DatumPointByCoordinate(coords)	This method creates a Feature object and a DatumPoint object at the point defined by the specified coordinates.
DatumPointByOffset(point, vector)	This method creates a Feature object and a DatumPoint object offset from an existing point by a vector.
DatumPointByMidPoint(point1, point2)	This method creates a Feature object and a DatumPoint object midway between two points.
DatumPointByOnFace(face, edge1, offset1, ...)	This method creates a Feature object and a DatumPoint object on the specified face, offset from two edges.
DatumPointByEdgeParam(edge, parameter)	This method creates a Feature object and a DatumPoint object along an edge at a selected distance from one end of the edge.
DatumPointByProjOnEdge(point, edge)	This method creates a Feature object and a DatumPoint object along an edge by projecting an existing point along the normal to the edge.
DatumPointByProjOnFace(point, face)	This method creates a Feature object and a DatumPoint object on a specified face by projecting an existing point onto the face.
MakeSketchTransform(sketchPlane[, origin, ...])	This method creates a Transform object.
PartitionCellByDatumPlane(cells, datumPlane)	This method partitions one or more cells using the given datum plane.
PartitionCellByExtendFace(cells, extendFace)	This method partitions one or more cells by extending the underlying geometry of a given face to partition the target cells.
PartitionCellByExtrudeEdge(cells, edges, ...)	This method partitions one or more cells by extruding selected edges in the given direction.
PartitionCellByPatchNCorners(cell, cornerPoints)	This method partitions a cell using an N-sided cutting patch defined by the given corner points.
PartitionCellByPatchNEdges(cell, edges)	This method partitions a cell using an N-sided cutting patch defined by the given edges.
PartitionCellByPlaneNormalToEdge(cells, ...)	This method partitions one or more cells using a plane normal to an edge at the given edge point.
PartitionCellByPlanePointNormal(cells, ...)	This method partitions one or more cells using a plane defined by a point and a normal direction.
PartitionCellByPlaneThreePoints(cells, ...)	This method partitions one or more cells using a plane defined by three points.
PartitionCellBySweepEdge(cells, edges, sweepPath)	This method partitions one or more cells by sweeping selected edges along the given sweep path.
PartitionEdgeByDatumPlane(edges, datumPlane)	This method partitions an edge where it intersects with a datum plane.
PartitionEdgeByParam(edges, parameter)	This method partitions one or more edges at the given normalized edge parameter.
PartitionEdgeByPoint(edge, point)	This method partitions an edge at the given point.
PartitionFaceByAuto(face)	This method automatically partitions a target face into simple regions that can be meshed using a structured meshing technique.
PartitionFaceByCurvedPathEdgeParams(face, ...)	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.
PartitionFaceByCurvedPathEdgePoints(face, ...)	This method partitions a face normal to two edges, using a curved path between the two given edge points.
PartitionFaceByDatumPlane(faces, datumPlane)	This method partitions one or more faces using the given datum plane.
PartitionFaceByExtendFace(faces, extendFace)	This method partitions one or more faces by extending the underlying geometry of another given face to partition the target faces.
PartitionFaceByIntersectFace(faces, cuttingFaces)	This method partitions one or more faces using the given cutting faces to partition the target faces.
PartitionFaceByProjectingEdges(faces, edges)	This method partitions one or more faces by projecting the given edges on the target faces.
PartitionFaceByShortestPath(faces, point1, ...)	This method partitions one or more faces using a minimum distance path between the two given points.
PartitionFaceBySketch(faces, sketch[, ...])	This method partitions one or more planar faces by sketching on them.
PartitionFaceBySketchDistance(faces, ...[, ...])	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.
PartitionFaceBySketchRefPoint(faces, ...[, ...])	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.
PartitionFaceBySketchThruAll(faces, ...[, ...])	This method partitions one or more faces by sketching on a sketch plane and then projecting toward the target faces through an infinite distance.
ReferencePoint(point[, instanceName])	This method creates a Feature object and a ReferencePoint object at the specified location.
RemoveWireEdges(wireEdgeList)	This method removes wire edges.
WirePolyLine(points[, mergeType, meshable])	This method creates an additional Feature object by creating a series of wires joining points in pairs.
isSuppressed()	This method queries the suppressed state of the feature.
restore()	This method restores the parameters of all features in the assembly to the value they had before a failed regeneration.
resume()	This method resumes suppressed features.
setValues(regenerateConstraintsTogether)	This method modifies the behavior associated with the specified assembly.
suppress()	This method suppresses features.

---

assignStackDirection(cells, referenceRegion)

This method assigns a stack direction to geometric cells. The stack direction will be used to orient the elements during mesh generation.

Note

Check MeshAssembly.assignStackDirection on help.3ds.com/0.1..

Parameters:

• cells (Tuple[Cell, ...]) – A sequence of Cell objects specifying regions where to assign the stack direction.

• referenceRegion (Face) – A Face object specifying the top side of the stack direction.

associateMeshWithGeometry(geometricEntity, elements=(), elemFaces=(), elemEdges=(), node=<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.

Note

Check MeshAssembly.associateMeshWithGeometry on help.3ds.com/0.1..

Parameters:

• geometricEntity (str) – 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 (Tuple[MeshElement, ...], default: ()) – A sequence of MeshElement objects specifying the elements to be associated with the geometric cell.

• elemFaces (Tuple[MeshFace, ...], default: ()) – A sequence of MeshFace objects specifying the element faces to be associated with the geometric face.

• elemEdges (Tuple[MeshEdge, ...], default: ()) – A sequence of MeshEdge objects specifying the element edges to be associated with the geometric edge.

• node (MeshNode, default: <abaqus.Mesh.MeshNode.MeshNode object at 0x7f350e0ff820>) – A MeshNode object specifying the mesh node to be associated with the geometric vertex.

createVirtualTopology(regions, mergeShortEdges=False, shortEdgeThreshold=None, mergeSmallFaces=False, smallFaceAreaThreshold=None, mergeSliverFaces=False, faceAspectRatioThreshold=None, mergeSmallAngleFaces=False, smallFaceCornerAngleThreshold=None, mergeThinStairFaces=False, thinStairFaceThreshold=None, ignoreRedundantEntities=False, cornerAngleTolerance=30, applyBlendControls=False, blendSubtendedAngleTolerance=None, blendRadiusTolerance=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.

Note

Check MeshAssembly.createVirtualTopology on help.3ds.com/0.1..

Parameters:

• regions (Tuple[Face, ...]) – A sequence of Face objects or PartInstance 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.

• mergeShortEdges (Union[AbaqusBoolean, bool], default: False) – A Boolean specifying whether to merge short edges. The default value is False.

• shortEdgeThreshold (Optional[float], default: None) – 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 (Union[AbaqusBoolean, bool], default: False) – A Boolean specifying whether to merge faces with small area. The default value is False.

• smallFaceAreaThreshold (Optional[float], default: None) – 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 (Union[AbaqusBoolean, bool], default: False) – A Boolean specifying whether to merge faces with high aspect ratio. The default value is False.

• faceAspectRatioThreshold (Optional[float], default: None) – A Float specifying a threshold that determines which faces are considered to have high aspect ratio. These faces are 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 (Union[AbaqusBoolean, bool], default: False) – A Boolean specifying whether to merge faces that have a sharp corner angle. The default value is False.

• smallFaceCornerAngleThreshold (Optional[float], default: None) – 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 (Union[AbaqusBoolean, bool], default: False) – A Boolean specifying whether to merge faces that represent a thin stair-like feature. The default value is False.

• thinStairFaceThreshold (Optional[float], default: None) – 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 (Union[AbaqusBoolean, bool], default: False) – A Boolean specifying whether to abstract away redundant edges and vertices. The default value is False.

• cornerAngleTolerance (float, default: 30) – 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 (Union[AbaqusBoolean, bool], default: False) – 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 (Optional[float], default: None) – 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 (Optional[float], default: None) – 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 – A Feature object

Return type:

Feature

deleteBoundaryLayerControls(regions)

This method deletes the control parameters for boundary layer mesh for all the specified regions.

Note

Check MeshAssembly.deleteBoundaryLayerControls on help.3ds.com/0.1..

Parameters:

regions (Tuple[Cell, ...]) – A sequence of Cell objects specifying the regions for which to set the boundary layer mesh control parameters.

deleteMesh(regions)

This method deletes a subset of the mesh that contains the native elements from the given part instances or regions.

Note

Check MeshAssembly.deleteMesh on help.3ds.com/0.1..

Parameters:

regions (Tuple[PartInstance, ...]) – A sequence of PartInstance objects or Region objects specifying the part instances or regions from where the native mesh is to be deleted.

deleteMeshAssociationWithGeometry(geometricEntities, addBoundingEntities=False)

This method deletes the association of geometric entities with mesh entities.

Note

Check MeshAssembly.deleteMeshAssociationWithGeometry on help.3ds.com/0.1..

Parameters:

• geometricEntities (Tuple[Cell, ...]) – A sequence of Cell objects, Face objects, Edge objects, or ConstrainedSketchVertex objects specifying the geometric entities that will be disassociated from the mesh.

• addBoundingEntities (Union[AbaqusBoolean, bool], default: False) – 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.

deletePreviewMesh()

This method deletes all boundary meshes in the assembly. See the boundaryPreview argument of generateMesh for information about generating boundary meshes.

deleteSeeds(regions)

This method deletes the global edge seeds from the given part instances or deletes the local edge seeds from the given edges.

Note

Check MeshAssembly.deleteSeeds on help.3ds.com/0.1..

Parameters:

regions (Tuple[PartInstance, ...]) – A sequence of PartInstance objects or Edge objects specifying the part instances or edges from which the seeds are to be deleted.

generateBottomUpExtrudedMesh(cell, numberOfLayers, extrudeVector, geometrySourceSide='', elemFacesSourceSide=(), elemSourceSide=(), depth=None, targetSide='', biasRatio=1, extendElementSets=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.

Note

Check MeshAssembly.generateBottomUpExtrudedMesh on help.3ds.com/0.1..

Parameters:

• cell (Cell) – A Cell object specifying the geometric region where the mesh is to be generated. This argument is valid only for native part instances.

• numberOfLayers (int) – An Int specifying the number of layers to be generated along the extrusion vector.

• extrudeVector (tuple) – 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 (str, default: '') – A Region of Face objects specifying the geometric domain to be used as the source for the extrude meshing operation.

• elemFacesSourceSide (Tuple[MeshFace, ...], default: ()) – A sequence of MeshFace objects specifying the faces of 3D elements to be used as the source for the extrude meshing operation.

• elemSourceSide (tuple, default: ()) – A sequence of 2D MeshElement objects specifying the elements to be used as the source for the extrude meshing operation.

• depth (Optional[float], default: None) – A Float specifying the distance of the mesh extrusion. If unspecified, the vector length of the extrudeVector argument is assumed.

• targetSide (str, default: '') – 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 (float, default: 1) – 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 (Union[AbaqusBoolean, bool], default: False) – 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 part instances. The default value is False.

generateBottomUpRevolvedMesh(cell, numberOfLayers, axisOfRevolution, angleOfRevolution, geometrySourceSide='', elemFacesSourceSide=(), elemSourceSide=(), extendElementSets=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.

Note

Check MeshAssembly.generateBottomUpRevolvedMesh on help.3ds.com/0.1..

Parameters:

• cell (Cell) – A Cell object specifying the geometric region where the mesh is to be generated. This argument is valid only for native part instances.

• numberOfLayers (int) – An Int specifying the number of layers of elements to be generated around the axis of revolution.

• axisOfRevolution (tuple) – 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 (float) – A Float specifying the angle of revolution.

• geometrySourceSide (str, default: '') – A Region of Face objects specifying the geometric domain to be used as the source for the revolve meshing operation.

• elemFacesSourceSide (Tuple[MeshFace, ...], default: ()) – A sequence of MeshFace objects specifying the faces of 3D elements to be used as the source for the revolve meshing operation.

• elemSourceSide (tuple, default: ()) – A sequence of 2D MeshElement objects specifying the elements to be used as the source for the revolve meshing operation.

• extendElementSets (Union[AbaqusBoolean, bool], default: False) – 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 part instances. The default value is False.

generateBottomUpSweptMesh(cell, geometrySourceSide='', elemFacesSourceSide=(), elemSourceSide=(), geometryConnectingSides='', elemFacesConnectingSides=(), elemConnectingSides=(), targetSide=None, numberOfLayers=None, extendElementSets=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.

Note

Check MeshAssembly.generateBottomUpSweptMesh on help.3ds.com/0.1..

Parameters:

• cell (Cell) – A Cell object specifying the geometric region where the mesh is to be generated. This argument is valid only for native part instances.

• geometrySourceSide (str, default: '') – A Region of Face objects specifying the geometric domain to be used as the source for the sweep meshing operation.

• elemFacesSourceSide (Tuple[MeshFace, ...], default: ()) – A sequence of MeshFace objects specifying the faces of 3D elements to be used as the source for the sweep meshing operation.

• elemSourceSide (tuple, default: ()) – A sequence of 2D MeshElement objects specifying the elements to be used as the source for the sweep meshing operation.

• geometryConnectingSides (str, default: '') – A Region of Face objects specifying the connecting sides of the sweep meshing operation.

• elemFacesConnectingSides (Tuple[MeshFace, ...], default: ()) – A sequence of MeshFace objects specifying connecting sides of the sweep meshing operation.

• elemConnectingSides (tuple, default: ()) – A sequence of 2D MeshElement objects specifying connecting sides of the sweep meshing operation.

• targetSide (Optional[Face], default: None) – A Face object specifying the target side of the sweep meshing operation.

• numberOfLayers (Optional[int], default: None) – An Int specifying the number of layers to be generated along the sweep direction.

• extendElementSets (Union[AbaqusBoolean, bool], default: False) – 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 part instances. The default value is False.

generateMesh(regions=(), seedConstraintOverride=OFF, meshTechniqueOverride=OFF, boundaryPreview=OFF, boundaryMeshOverride=OFF)

This method generates a mesh in the given part instances or regions.

Note

Check MeshAssembly.generateMesh on help.3ds.com/0.1..

Parameters:

• regions (Tuple[PartInstance, ...], default: ()) – A sequence of PartInstance objects or Region objects specifying the part instances or regions where the mesh is to be generated.

• seedConstraintOverride (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether mesh generation is allowed to modify seed constraints. The default value is OFF.

• meshTechniqueOverride (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether mesh generation is allowed to modify the existing mesh techniques so that a compatible mesh can be generated. The default value is OFF.

• boundaryPreview (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the generated mesh should be a boundary mesh. This option will only have an effect if any of the specified regions are to be meshed with tetrahedral elements or using the bottom-up technique with hexahedral or wedge elements. The default value is OFF.

• boundaryMeshOverride (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether mesh generation is allowed to modify an existing boundary preview mesh. This option will only have an effect if any of the specified regions are to be meshed with tetrahedral elements and a boundary preview mesh already exists. The default value is OFF.

getEdgeSeeds(edge, attribute)

This method returns an edge seed parameter for a specified edge of an assembly.

Note

Check MeshAssembly.getEdgeSeeds on help.3ds.com/0.1..

Parameters:

• edge (Edge) – An Edge object specifying the edge to be queried.

• attribute (Union[SymbolicConstant, float]) –

  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

Returns:

The return value is a Float, an Int, or a SymbolicConstant depending on the value of the attribute argument.

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.

Return type:

Union[float, int, SymbolicConstant]

getElementType(region, elemShape)

This method returns the ElemType object of a given element shape assigned to a region of the assembly.

Note

Check MeshAssembly.getElementType on help.3ds.com/0.1..

Parameters:

• region (str) – A Cell, a Face, or an Edge object specifying the region to be queried.

• elemShape (SymbolicConstant) – A SymbolicConstant specifying the shape of the element for which to return the element type. Possible values are:LINEQUADTRIHEXWEDGETET

Returns:

An ElemType object.

Return type:

ElementType

Raises:

TypeError – If the region cannot be associated with element types or if the elemShape is not consistent with the dimension of the region.

getIncompatibleMeshInterfaces(cells=())

This method returns a sequence of face objects that are meshed with incompatible elements.

Note

Check MeshAssembly.getIncompatibleMeshInterfaces on help.3ds.com/0.1..

Parameters:

cells (Tuple[Cell, ...], default: ()) – A sequence of Cell objects which will be used to search the incompatible faces.

Returns:

A sequence of Face objects.

Return type:

Tuple[Face, ]

getMeshControl(region, attribute)

This method returns a mesh control parameter for the specified region of the assembly.

Note

Check MeshAssembly.getMeshControl on help.3ds.com/0.1..

Parameters:

• region (str) – A Cell, a Face, or an Edge object specifying the region to be queried.

• attribute (SymbolicConstant) –

  A SymbolicConstant specifying the mesh control attribute to return. Possible values are:

  • ELEM_SHAPE

  • TECHNIQUE

  • ALGORITHM

  • MIN_TRANSITION

  The return value is dependent on 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.

Return type:

Union[bool, SymbolicConstant]

Raises:

TypeError – The region cannot carry mesh controls.

getMeshStats(regions)

This method returns the mesh statistics for the given part instances or regions.

Note

Check MeshAssembly.getMeshStats on help.3ds.com/0.1..

Parameters:

regions (tuple) – A sequence or tuple of PartInstance objects or ConstrainedSketchGeometry regions for which mesh statistics should be returned.

Returns:

A MeshStats object.

Return type:

MeshStats

getPartSeeds(region, attribute)

This method returns a part seed parameter for the specified instance.

Note

Check MeshAssembly.getPartSeeds on help.3ds.com/0.1..

Parameters:

• region (PartInstance) – A PartInstance object specifying the part instance to be queried.

• attribute (Union[SymbolicConstant, float]) –

  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 is dependent 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, and its value is dependent on the attribute argument.

Return type:

float

Raises:

Error – An exception occurs if the part instance does not contain native geometry.

getUnmeshedRegions()

This method returns all geometric regions in the assembly that require a mesh for submitting an analysis but are either unmeshed or are meshed incompletely.

Returns:

A Region object, or None.

Return type:

Region

ignoreEntity(entities)

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.

Note

Check MeshAssembly.ignoreEntity on help.3ds.com/0.1..

Parameters:

entities (tuple) – A sequence of vertices and edges specifying the entities to be ignored during meshing.

Returns:

feature – A Feature object

Return type:

Feature

restoreIgnoredEntity(entities)

This method restores vertices and edges that have been merged using a virtual topology feature.

Note

Check MeshAssembly.restoreIgnoredEntity on help.3ds.com/0.1..

Parameters:

entities (Tuple[IgnoredVertex, ...]) – A sequence of IgnoredVertex objects and IgnoredEdge objects specifying the entities to be restored.

Returns:

feature – A Feature object

Return type:

Feature

seedEdgeByBias(biasMethod, end1Edges, end2Edges, centerEdges, endEdges, ratio, number, minSize, maxSize, constraint=abaqusConstants.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.

Note

Check MeshAssembly.seedEdgeByBias on help.3ds.com/0.1..

Parameters:

• biasMethod (SymbolicConstant) – 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 (Tuple[Edge, ...]) – 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 (Tuple[Edge, ...]) – 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 (Tuple[Edge, ...]) – 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 (Tuple[Edge, ...]) – A sequence of Edge objects specifying the edges to seed. The smallest elements will be positioned near edge ends.

• ratio (float) – A Float specifying the ratio of the largest element to the smallest element. Possible values are 1.0 ≤ ratio ≤ 106.

• number (int) – An Int specifying the number of elements along each edge. Possible values are 1 ≤ number ≤ 104.

• minSize (float) – A Float specifying the desired smallest element size.

• maxSize (float) – 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 (SymbolicConstant, default: FREE) –

  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, number, constraint=abaqusConstants.FREE)

This method seeds the given edges uniformly based on the number of elements along the edges.

Note

Check MeshAssembly.seedEdgeByNumber on help.3ds.com/0.1..

Parameters:

• edges (Tuple[Edge, ...]) – A sequence of Edge objects specifying the edges to seed.

• number (int) – An Int specifying the number of elements along each edge. Possible values are 1 ≤ number ≤ 104.

• constraint (SymbolicConstant, default: FREE) – 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, size, deviationFactor=None, minSizeFactor=None, constraint=abaqusConstants.FREE)

This method seeds the given edges either uniformly or following edge curvature distribution, based on the desired element size.

Note

Check MeshAssembly.seedEdgeBySize on help.3ds.com/0.1..

Parameters:

• edges (Tuple[Edge, ...]) – A sequence of Edge objects specifying the edges to seed.

• size (float) – A Float specifying the desired element size.

• deviationFactor (Optional[float], default: None) – A Float specifying the deviation factor h/Lh/L, where hh is the chordal deviation and LL is the element length.

• minSizeFactor (Optional[float], default: None) – A Float specifying the size of the smallest allowable element as a fraction of the specified global element size.

• constraint (SymbolicConstant, default: FREE) – 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).

seedPartInstance(regions, size, deviationFactor=None, minSizeFactor=None, constraint=abaqusConstants.FREE)

This method assigns global edge seeds to the given part instances.

Note

Check MeshAssembly.seedPartInstance on help.3ds.com/0.1..

Parameters:

• regions (Tuple[PartInstance, ...]) – A sequence of PartInstance objects specifying the part instances to seed.

• size (float) – A Float specifying the desired global element size for the edges.

• deviationFactor (Optional[float], default: None) – A Float specifying the deviation factor h/Lh/L, where hh is the chordal deviation and LL is the element length.

• minSizeFactor (Optional[float], default: None) – A Float specifying the size of the smallest allowable element as a fraction of the specified global element size.

• constraint (SymbolicConstant, default: FREE) – 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.

setBoundaryLayerControls(regions, firstElemSize, growthFactor, numLayers, inactiveFaces=(), setName='')

This method sets the control parameters for boundary layer mesh for the specified regions.

Note

Check MeshAssembly.setBoundaryLayerControls on help.3ds.com/0.1..

Parameters:

• regions (Tuple[Cell, ...]) – A sequence of Cell objects specifying the regions for which to set the boundary layer mesh control parameters.

• firstElemSize (float) – A Float specifying the height of the first element layer off boundary. Possible values are 0.0 << firstElemSize ≤ 106.

• growthFactor (float) – A Float specifying the ratio of heights of any two consecutive element layers. Possible values are 1.0 ≤ growthFactor ≤ 10.0.

• numLayers (int) – An Int specifying the number of element layers to be generated. Possible values are 1 ≤ numLayers ≤ 104.

• inactiveFaces (Tuple[Face, ...], default: ()) – 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 (str, default: '') – A String specifying a unique name for a set that will contain boundary layer elements.

setElementType(regions, elemTypes)

This method assigns element types to the specified regions.

Note

Check MeshAssembly.setElementType on help.3ds.com/0.1..

Parameters:

• regions (tuple) – 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 (Tuple[ElemType, ...]) – 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:

Exception – 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, corners)

This method sets the logical corners for a mappable face region.

Note

Check MeshAssembly.setLogicalCorners on help.3ds.com/0.1..

Parameters:

• region (str) – A Face region.

• corners (str) – Three, four, or five ConstrainedSketchVertex objects defining the logical corners for a given mappable face region.

setMeshControls(regions, elemShape=None, technique=None, algorithm=None, minTransition=ON, sizeGrowth=None, allowMapped=OFF)

This method sets the mesh control parameters for the specified regions.

Note

Check MeshAssembly.setMeshControls on help.3ds.com/0.1..

Parameters:

• regions (tuple) – A sequence of Face or Cell regions specifying the regions for which to set the mesh control parameters.

• elemShape (Optional[SymbolicConstant], default: None) –

  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 (Optional[SymbolicConstant], default: None) –

  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 (Optional[SymbolicConstant], default: None) –

  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 tetrahedral-meshing technique will be used.

• minTransition (Union[AbaqusBoolean, bool], default: ON) –

  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 (Optional[SymbolicConstant], default: None) – 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 (Union[AbaqusBoolean, bool], default: OFF) –

  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, edge, sense)

This method sets the sweep path for a sweepable region or the revolve path for a revolvable region.

Note

Check MeshAssembly.setSweepPath on help.3ds.com/0.1..

Parameters:

• region (str) – A sweepable region.

• edge (Edge) – An Edge object specifying the sweep or revolve path.

• sense (SymbolicConstant) – 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.

verifyMeshQuality(criterion, threshold=None, elemShape=None, regions=())

This method tests the quality of part instance meshes and returns poor-quality elements.

Note

Check MeshAssembly.verifyMeshQuality on help.3ds.com/0.1..

Parameters:

• criterion (SymbolicConstant) –

  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 (Optional[float], default: None) – 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 (Optional[SymbolicConstant], default: None) – A SymbolicConstant specifying an element shape for limiting the query. Possible values are LINE, QUAD, TRI, HEX, WEDGE, and TET.

• regions (tuple, default: ()) – A sequence of Region or MeshElement objects. If you do not specify the regions argument, all meshes in the assembly are 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) .

Return type:

Dict[str, int | float | MeshElement]

ElemType

class ElemType(elemCode, elemLibrary=abaqusConstants.STANDARD, hourglassStiffness=0, bendingHourglass=0, drillingHourglass=0, kinematicSplit=abaqusConstants.AVERAGE_STRAIN, distortionControl=OFF, lengthRatio=ON, secondOrderAccuracy=OFF, hourglassControl=abaqusConstants.ENHANCED, weightFactor=0, displacementHourglass=1, rotationalHourglass=1, outOfPlaneDisplacementHourglass=1, elemDeletion=abaqusConstants.DEFAULT, particleConversion=abaqusConstants.DEFAULT, particleConversionThreshold=0, particleConversionPPD=1, particleConversionKernel=abaqusConstants.CUBIC, maxDegradation=None, viscosity=0, linearBulkViscosity=1, quadraticBulkViscosity=1, numFourierModes=1, nodeOffset=None, linearKinematicCtrl=None, initialGapOpening=None)

The ElemType object is an argument object used as an argument in the setElementType command.

Note

This object can be accessed by:

import mesh

Note

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

Public Data Attributes:

elemLibrary	A SymbolicConstant specifying the Abaqus element library to use.
hourglassStiffness	A Float specifying the hourglass stiffness.
bendingHourglass	A Float specifying the bending hourglass stiffness.
drillingHourglass	A Float specifying the drilling hourglass scaling factor.
kinematicSplit	A SymbolicConstant specifying the kinematic split control.
distortionControl	A Boolean specifying whether to prevent negative element volumes or other excessive distortions in crushable materials.
lengthRatio	A Float specifying the length ratio for distortion control in crushable materials.
secondOrderAccuracy	A Boolean specifying the second-order accuracy option.
hourglassControl	A SymbolicConstant specifying the hourglass control.
weightFactor	A Float specifying a weight factor when hourglassControl = COMBINED.
displacementHourglass	A Float specifying the displacement hourglass scaling factor.
rotationalHourglass	A Float specifying the rotational hourglass scaling factor.
outOfPlaneDisplacementHourglass	A Float specifying the out-of-plane displacement hourglass scaling factor.
elemDeletion	A SymbolicConstant specifying the element deletion option.
particleConversion	A SymbolicConstant specifying the particle conversion option for smoothed particle hydrodynamics.
particleConversionThreshold	A Float specifying the threshold value for the particle conversion criterion specified by particleConversion.
particleConversionPPD	An Int specifying the number of particles per direction for element conversion when particleConversion is specified.
particleConversionKernel	A SymbolicConstant specifying the interpolation function for particle conversion when particleConversion is specified.
maxDegradation	A Float specifying the maximum degradation option for damage control.
viscosity	A Float specifying the viscosity option.
linearBulkViscosity	A Float specifying the linear bulk viscosity scaling factor option for Abaqus/Explicit.
quadraticBulkViscosity	A Float specifying the quadratic bulk viscosity scaling factor option for Abaqus/Explicit.
numFourierModes	An Int specifying the number of Fourier modes.
nodeOffset	An Int specifying the positive offset number for specifying the additional nodes needed in the connectivity.This argument is applicable only for axisymmetric elements with nonlinear asymmetric deformation.
linearKinematicCtrl	A Float specifying the linear kinematic conversion value.This argument is applicable only to some Abaqus/Explicit elements.
initialGapOpening	A Float specifying the initial gap opening.This parameter is applicable only to some Abaqus/Standard elements.

Public Methods:

__init__(elemCode[, elemLibrary, ...])

This method creates an ElemType object.

---

bendingHourglass: float = 0

A Float specifying the bending hourglass stiffness. A value of zero indicates the default value should be used. The default value will be used where appropriate. The default value is 0.0.This argument is applicable only to some Abaqus/Standard elements.

displacementHourglass: float = 1

A Float specifying the displacement hourglass scaling factor. The default value will be used where appropriate. The default value is 1.0.This argument is applicable only to some Abaqus/Explicit elements.

distortionControl: Union[AbaqusBoolean, bool] = OFF

A Boolean specifying whether to prevent negative element volumes or other excessive distortions in crushable materials. The default value is OFF.This argument is applicable only to some Abaqus/Explicit elements.

drillingHourglass: float = 0

A Float specifying the drilling hourglass scaling factor. A value of zero indicates the default value should be used. The default value will be used where appropriate. The default value is 0.0.This argument is applicable only to some Abaqus/Standard elements.

elemCode: SymbolicConstant

A SymbolicConstant specifying the Abaqus element code or just the element shape. Possible values are:

• C3D8R, specifying a 8-node linear brick, reduced integration with hourglass control.

• CODE, specifying add more codes.

• UNKNOWN_TRI, specifying an unknown element type associated with a triangular shape.

• UNKNOWN_QUAD, specifying an unknown element type associated with a quadrilateral shape.

• UNKNOWN_HEX, specifying an unknown element type associated with a hexahedral shape.

• UNKNOWN_WEDGE, specifying an unknown element type associated with a wedge shape.

• UNKNOWN_TET, specifying an unknown element type associated with a tetrahedral shape.

elemDeletion: SymbolicConstant = DEFAULT

A SymbolicConstant specifying the element deletion option. Possible values are DEFAULT, ON, and OFF. The default value is DEFAULT.

elemLibrary: SymbolicConstant = STANDARD

A SymbolicConstant specifying the Abaqus element library to use. Possible values are STANDARD and EXPLICIT. The default value is STANDARD.

hourglassControl: SymbolicConstant = ENHANCED

A SymbolicConstant specifying the hourglass control. Possible values are RELAX_STIFFNESS, STIFFNESS, VISCOUS, ENHANCED, and COMBINED. The default value is ENHANCED.This argument is applicable only to some Abaqus/Explicit elements.

hourglassStiffness: float = 0

A Float specifying the hourglass stiffness. (For shell elements this is the membrane hourglass stiffness.) A value of zero indicates the default value should be used. The default value will be used where appropriate. The default value is 0.0.This argument is applicable only to some Abaqus/Standard elements.

initialGapOpening: Optional[float] = None

A Float specifying the initial gap opening.This parameter is applicable only to some Abaqus/Standard elements.

New in version 2022: The initialGapOpening attribute was added.

kinematicSplit: SymbolicConstant = AVERAGE_STRAIN

A SymbolicConstant specifying the kinematic split control. Possible values are AVERAGE_STRAIN, ORTHOGONAL, and CENTROID. The default value is AVERAGE_STRAIN.This argument is applicable only to some Abaqus/Explicit elements.

lengthRatio: float = ON

A Float specifying the length ratio for distortion control in crushable materials. Possible values are 0.0 ≤ lengthRatio ≤ 1.0. The default value is lengthRatio = 0.10.1This argument is applicable only when distortionControl is ON.

linearBulkViscosity: float = 1

A Float specifying the linear bulk viscosity scaling factor option for Abaqus/Explicit. The default value is 1.0.

linearKinematicCtrl: Optional[float] = None

A Float specifying the linear kinematic conversion value.This argument is applicable only to some Abaqus/Explicit elements.

New in version 2022: The linearKinematicCtrl attribute was added.

maxDegradation: Optional[float] = None

A Float specifying the maximum degradation option for damage control. The default value is −1.0.

nodeOffset: Optional[int] = None

An Int specifying the positive offset number for specifying the additional nodes needed in the connectivity.This argument is applicable only for axisymmetric elements with nonlinear asymmetric deformation.

New in version 2019: The nodeOffset attribute was added.

numFourierModes: int = 1

An Int specifying the number of Fourier modes. Possible values are 1, 2, 3, and 4. The default value is 1.This argument is applicable only for axisymmetric elements with nonlinear asymmetric deformation.

New in version 2019: The numFourierModes attribute was added.

outOfPlaneDisplacementHourglass: float = 1

A Float specifying the out-of-plane displacement hourglass scaling factor. The default value will be used where appropriate. The default value is 1.0.This argument is applicable only to some Abaqus/Explicit elements.

particleConversion: SymbolicConstant = DEFAULT

A SymbolicConstant specifying the particle conversion option for smoothed particle hydrodynamics. When not OFF or DEFAULT this argument refers to the criterion used for conversion of elements to particles. Possible values are DEFAULT, OFF, TIME, STRAIN, and STRESS. The default value is DEFAULT.This argument is applicable only to some Abaqus/Explicit elements.

particleConversionKernel: SymbolicConstant = CUBIC

A SymbolicConstant specifying the interpolation function for particle conversion when particleConversion is specified. Possible values are CUBIC, QUADRATIC, and QUINTIC. The default value is CUBIC.This argument is applicable only to some Abaqus/Explicit elements.

particleConversionPPD: int = 1

An Int specifying the number of particles per direction for element conversion when particleConversion is specified. The default value is 1.This argument is applicable only to some Abaqus/Explicit elements.

particleConversionThreshold: float = 0

A Float specifying the threshold value for the particle conversion criterion specified by particleConversion. The default value is 0.0.This argument is applicable only to some Abaqus/Explicit elements.

quadraticBulkViscosity: float = 1

A Float specifying the quadratic bulk viscosity scaling factor option for Abaqus/Explicit. The default value is 1.0.

rotationalHourglass: float = 1

A Float specifying the rotational hourglass scaling factor. The default value will be used where appropriate. The default value is 1.0.This argument is applicable only to some Abaqus/Explicit elements.

secondOrderAccuracy: Union[AbaqusBoolean, bool] = OFF

A Boolean specifying the second-order accuracy option. The default value is OFF.This argument is applicable only to some Abaqus/Explicit elements.

viscosity: float = 0

A Float specifying the viscosity option. The default value is 0.0.This argument is applicable only to some Abaqus/Standard elements.

weightFactor: float = 0

A Float specifying a weight factor when hourglassControl = COMBINED. The default value is 0.5.This argument is applicable only to some Abaqus/Explicit elements.

MeshEdge

class MeshEdge

The MeshEdge object refers to an element edge. It has no constructor or members. A MeshEdge object can be accessed via a MeshEdgeArray or a repository on a part or part instance.

Note

This object can be accessed by:

import part
mdb.models[name].parts[name].elemEdges[i]
mdb.models[name].parts[name].elementEdges[i]
import assembly
mdb.models[name].rootAssembly.allInstances[name].elemEdges[i]
mdb.models[name].rootAssembly.allInstances[name].elementEdges[i]
mdb.models[name].rootAssembly.instances[name].elemEdges[i]
mdb.models[name].rootAssembly.instances[name].elementEdges[i]

Note

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

Public Methods:

getElements()	This method returns a tuple of elements that share the element edge.
getElementsViaTopology([domain])	This method returns an array of MeshElement objects that are obtained by recursively finding adjacent elements via topology.
getNodesViaTopology([domain])	This method returns an array of MeshNode objects that lie along element edges topologically in line with the element edge.
getElemFaces()	This method returns a tuple of unique MeshFace objects that share the element edge.
getNodes()	This method returns a tuple of nodes on the element edge.

---

getElemFaces()

This method returns a tuple of unique MeshFace objects that share the element edge.

Returns:

A tuple of MeshFace objects.

Return type:

Tuple[MeshFace, ]

getElements()

This method returns a tuple of elements that share the element edge.

Returns:

A tuple of MeshElement objects.

Return type:

Tuple[MeshElement, ]

getElementsViaTopology(domain=[])

This method returns an array of MeshElement objects that are obtained by recursively finding adjacent elements via topology.

Note

Check MeshEdge.getElementsViaTopology on help.3ds.com/0.1..

Parameters:

domain (MeshElementArray, default: []) – A MeshElementArray object specifying the domain to include in the search. By default, all elements in the mesh are included.

Returns:

A MeshElementArray object, which is a sequence of MeshElement objects.

Return type:

MeshElementArray

getNodes()

This method returns a tuple of nodes on the element edge.

Returns:

A tuple of MeshNode objects.

Return type:

Tuple[MeshNode, ]

getNodesViaTopology(domain=[])

This method returns an array of MeshNode objects that lie along element edges topologically in line with the element edge.

Note

Check MeshEdge.getNodesViaTopology on help.3ds.com/0.1..

Parameters:

domain (MeshElementArray, default: []) – A MeshElementArray object specifying the domain to include in the search. By default, all elements in the mesh are included.

Returns:

A MeshNodeArray object, which is a sequence of MeshNode objects.

Return type:

MeshNodeArray

MeshEdgeArray

class MeshEdgeArray(elemEdges)

The MeshEdgeArray is a sequence of MeshEdge objects.

Note

This object can be accessed by:

import part
mdb.models[name].parts[name].elementEdges
import assembly
mdb.models[name].rootAssembly.allInstances[name].elementEdges
mdb.models[name].rootAssembly.instances[name].elementEdges

Note

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

Public Methods:

__init__(elemEdges)	This method creates a MeshEdgeArray object.
getSequenceFromMask(mask)	This method returns the objects in the MeshEdgeArray identified using the specified mask.
getMask()	This method returns a string specifying the object or objects.

Inherited from list

__repr__()	Return repr(self).
__getattribute__(name, /)	Return getattr(self, name).
__lt__(value, /)	Return self<value.
__le__(value, /)	Return self<=value.
__eq__(value, /)	Return self==value.
__ne__(value, /)	Return self!=value.
__gt__(value, /)	Return self>value.
__ge__(value, /)	Return self>=value.
__iter__()	Implement iter(self).
__init__(elemEdges)	This method creates a MeshEdgeArray object.
__len__()	Return len(self).
__getitem__	x.__getitem__(y) <==> x[y]
__setitem__(key, value, /)	Set self[key] to value.
__delitem__(key, /)	Delete self[key].
__add__(value, /)	Return self+value.
__mul__(value, /)	Return self*value.
__rmul__(value, /)	Return value*self.
__contains__(key, /)	Return key in self.
__iadd__(value, /)	Implement self+=value.
__imul__(value, /)	Implement self*=value.
__reversed__()	Return a reverse iterator over the list.
__sizeof__()	Return the size of the list in memory, in bytes.
clear()	Remove all items from list.
copy()	Return a shallow copy of the list.
append(object, /)	Append object to the end of the list.
insert(index, object, /)	Insert object before index.
extend(iterable, /)	Extend list by appending elements from the iterable.
pop([index])	Remove and return item at index (default last).
remove(value, /)	Remove first occurrence of value.
index(value[, start, stop])	Return first index of value.
count(value, /)	Return number of occurrences of value.
reverse()	Reverse IN PLACE.
sort(*[, key, reverse])	Sort the list in ascending order and return None.
__class_getitem__	See PEP 585

Inherited from Generic

__class_getitem__	See PEP 585
__init_subclass__(*args, **kwargs)	This method is called when a class is subclassed.

Private Data Attributes:

Inherited from Generic

_is_protocol

---

getMask()

This method returns a string specifying the object or objects.

Returns:

A String specifying the object or objects.

Return type:

str

getSequenceFromMask(mask)

This method returns the objects in the MeshEdgeArray identified using the specified mask. When large number of objects are involved, this method is highly efficient.

Note

Check MeshEdgeArray.getSequenceFromMask on help.3ds.com/0.1..

Parameters:

mask (str) – A String specifying the object or objects.

Returns:

A MeshEdgeArray object.

Return type:

MeshEdgeArray

Raises:

Error – An exception occurs if the resulting sequence is empty.

MeshElement

class MeshElement

The MeshElement object refers to an element of a native mesh or an orphan mesh. A MeshElement object can be accessed via a part or part instance using an index that refers to the internal numbering of the element repository. The index does not refer to the element label.

Note

This object can be accessed by:

import part
mdb.models[name].parts[name].allInternalSets[name].elements[i]
mdb.models[name].parts[name].allInternalSurfaces[name].elements[i]
mdb.models[name].parts[name].allSets[name].elements[i]
mdb.models[name].parts[name].allSurfaces[name].elements[i]
mdb.models[name].parts[name].elements[i]
mdb.models[name].parts[name].sets[name].elements[i]
mdb.models[name].parts[name].surfaces[name].elements[i]
import assembly
mdb.models[name].rootAssembly.allInstances[name].elements[i]
mdb.models[name].rootAssembly.allInstances[name].sets[name].elements[i]
mdb.models[name].rootAssembly.allInstances[name].surfaces[name].elements[i]
mdb.models[name].rootAssembly.allInternalSets[name].elements[i]
mdb.models[name].rootAssembly.allInternalSurfaces[name].elements[i]
mdb.models[name].rootAssembly.allSets[name].elements[i]
mdb.models[name].rootAssembly.allSurfaces[name].elements[i]
mdb.models[name].rootAssembly.elements[i]
mdb.models[name].rootAssembly.instances[name].elements[i]
mdb.models[name].rootAssembly.instances[name].sets[name].elements[i]
mdb.models[name].rootAssembly.instances[name].surfaces[name].elements[i]
mdb.models[name].rootAssembly.modelInstances[i].elements[i]
mdb.models[name].rootAssembly.modelInstances[i].sets[name].elements[i]
mdb.models[name].rootAssembly.modelInstances[i].surfaces[name].elements[i]
mdb.models[name].rootAssembly.sets[name].elements[i]
mdb.models[name].rootAssembly.surfaces[name].elements[i]

Note

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

Public Data Attributes:

label	An Int specifying the element label.
type	A SymbolicConstant specifying the Abaqus element code.
instanceName	A String specifying the name of the part instance that owns this element.
connectivity	A tuple of Ints specifying the internal node indices that define the nodal connectivity.

Public Methods:

Element(nodes, elemShape[, label])	This method creates an element on an orphan mesh part from a sequence of nodes.
getNodes()	This method returns a tuple of node objects of the element.
getElemEdges()	This method returns a tuple of unique element edge objects on the element.
getElemFaces()	This method returns a tuple of unique element face objects on the element.
getAdjacentElements()	This method returns an array of element objects adjacent to the mesh element.
getElementsByFeatureEdge(angle)	This method returns an array of mesh element objects that are obtained by recursively finding adjacent elements along a feature edge with a face angle of less than or equal to the specified angle.
setValues([label])	This method modifies the MeshElement object.

---

Element(nodes, elemShape, label=None)

This method creates an element on an orphan mesh part from a sequence of nodes.

Note

This function can be accessed by:

mdb.models[name].parts[name].Element

Note

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

Parameters:

• nodes (Tuple[MeshNode, ...]) – A sequence of MeshNode objects.

• elemShape (SymbolicConstant) – A SymbolicConstant specifying the shape of the new element. Possible values are LINE2, LINE3, TRI3, TRI6, QUAD4, QUAD8, TET4, TET10, WEDGE6, WEDGE15, HEX8, and HEX20.

• label (Optional[int], default: None) – An Int specifying the element label.

Returns:

element – A MeshElement object.

Return type:

MeshElement

connectivity: Optional[int] = None

A tuple of Ints specifying the internal node indices that define the nodal connectivity. It is important to note the difference with OdbMeshElement object of ODB where the connectivity is node labels instead of node indices.

getAdjacentElements()

This method returns an array of element objects adjacent to the mesh element.

Returns:

A MeshElementArray object which is a sequence of MeshElement objects.

Return type:

MeshElementArray

getElemEdges()

This method returns a tuple of unique element edge objects on the element.

Returns:

A tuple of MeshEdge objects.

Return type:

Tuple[MeshEdge, ]

getElemFaces()

This method returns a tuple of unique element face objects on the element.

Returns:

A tuple of MeshFace objects.

Return type:

Tuple[MeshFace, ]

getElementsByFeatureEdge(angle)

This method returns an array of mesh element objects that are obtained by recursively finding adjacent elements along a feature edge with a face angle of less than or equal to the specified angle.

Note

Check MeshElement.getElementsByFeatureEdge on help.3ds.com/0.1..

Parameters:

angle (str) – A float specifying the value of the face angle in degrees.

Returns:

A MeshElementArray object, which is a sequence of MeshElement objects.

Return type:

MeshElementArray

getNodes()

This method returns a tuple of node objects of the element.

Returns:

A tuple of MeshNode objects.

Return type:

Tuple[MeshNode, ]

instanceName: str = ''

A String specifying the name of the part instance that owns this element.

label: Optional[int] = None

An Int specifying the element label.

setValues(label=None)

This method modifies the MeshElement object.

Note

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

Parameters:

label (Optional[int], default: None) – An Int specifying the element label. This member may only be edited if the element belongs to an orphan mesh part. The specified label must be non-negative and must not be in use by any other element of the same part.

type: Optional[SymbolicConstant] = None

A SymbolicConstant specifying the Abaqus element code.

MeshElementArray

class MeshElementArray(elements)

The MeshElementArray is a sequence of MeshElement objects.

Note

This object can be accessed by:

import part
mdb.models[name].parts[name].allInternalSets[name].elements
mdb.models[name].parts[name].allInternalSurfaces[name].elements
mdb.models[name].parts[name].allSets[name].elements
mdb.models[name].parts[name].allSurfaces[name].elements
mdb.models[name].parts[name].elements
mdb.models[name].parts[name].sets[name].elements
mdb.models[name].parts[name].surfaces[name].elements
import assembly
mdb.models[name].rootAssembly.allInstances[name].elements
mdb.models[name].rootAssembly.allInstances[name].sets[name].elements
mdb.models[name].rootAssembly.allInstances[name].surfaces[name].elements
mdb.models[name].rootAssembly.allInternalSets[name].elements
mdb.models[name].rootAssembly.allInternalSurfaces[name].elements
mdb.models[name].rootAssembly.allSets[name].elements
mdb.models[name].rootAssembly.allSurfaces[name].elements
mdb.models[name].rootAssembly.elements
mdb.models[name].rootAssembly.instances[name].elements
mdb.models[name].rootAssembly.instances[name].sets[name].elements
mdb.models[name].rootAssembly.instances[name].surfaces[name].elements
mdb.models[name].rootAssembly.modelInstances[i].elements
mdb.models[name].rootAssembly.modelInstances[i].sets[name].elements
mdb.models[name].rootAssembly.modelInstances[i].surfaces[name].elements
mdb.models[name].rootAssembly.sets[name].elements
mdb.models[name].rootAssembly.surfaces[name].elements

Note

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

Public Methods:

__init__(elements)	This method creates a MeshElementArray object.
getFromLabel(label)	This method returns the object in the MeshElementArray with the given label.
getSequenceFromMask(mask)	This method returns the objects in the MeshElementArray identified using the specified mask.
getMask()	This method returns a string specifying the object or objects.
getByBoundingBox([xMin, yMin, zMin, xMax, ...])	This method returns an array of element objects that lie within the specified bounding box.
getByBoundingCylinder(center1, center2, radius)	This method returns an array of element objects that lie within the specified bounding cylinder.
getByBoundingSphere(center, radius)	This method returns an array of element objects that lie within the specified bounding sphere.
getBoundingBox()	This method returns a dictionary of two tuples representing minimum and maximum boundary values of the bounding box of the minimum size containing the element sequence.
sequenceFromLabels(labels)	This method returns the objects in the MeshElementArray identified using the specified labels.
getExteriorEdges()	This method returns the edges on the exterior of the faces in the FaceArray.
getExteriorFaces()	This method returns the cell faces on the exterior of the CellArray.

Inherited from list

__repr__()	Return repr(self).
__getattribute__(name, /)	Return getattr(self, name).
__lt__(value, /)	Return self<value.
__le__(value, /)	Return self<=value.
__eq__(value, /)	Return self==value.
__ne__(value, /)	Return self!=value.
__gt__(value, /)	Return self>value.
__ge__(value, /)	Return self>=value.
__iter__()	Implement iter(self).
__init__(elements)	This method creates a MeshElementArray object.
__len__()	Return len(self).
__getitem__	x.__getitem__(y) <==> x[y]
__setitem__(key, value, /)	Set self[key] to value.
__delitem__(key, /)	Delete self[key].
__add__(value, /)	Return self+value.
__mul__(value, /)	Return self*value.
__rmul__(value, /)	Return value*self.
__contains__(key, /)	Return key in self.
__iadd__(value, /)	Implement self+=value.
__imul__(value, /)	Implement self*=value.
__reversed__()	Return a reverse iterator over the list.
__sizeof__()	Return the size of the list in memory, in bytes.
clear()	Remove all items from list.
copy()	Return a shallow copy of the list.
append(object, /)	Append object to the end of the list.
insert(index, object, /)	Insert object before index.
extend(iterable, /)	Extend list by appending elements from the iterable.
pop([index])	Remove and return item at index (default last).
remove(value, /)	Remove first occurrence of value.
index(value[, start, stop])	Return first index of value.
count(value, /)	Return number of occurrences of value.
reverse()	Reverse IN PLACE.
sort(*[, key, reverse])	Sort the list in ascending order and return None.
__class_getitem__	See PEP 585

Inherited from Generic

__class_getitem__	See PEP 585
__init_subclass__(*args, **kwargs)	This method is called when a class is subclassed.

Private Data Attributes:

Inherited from Generic

_is_protocol

---

getBoundingBox()

This method returns a dictionary of two tuples representing minimum and maximum boundary values of the bounding box of the minimum size containing the element sequence.

Returns:

A Dictionary object with the following items:

• low: a tuple of three floats representing the minimum x, y, and z boundary values of the bounding box.

• high: a tuple of three floats representing the maximum x, y, and z boundary values of the bounding box.

Return type:

Dict[str, Tuple[float, float, float]]

getByBoundingBox(xMin=Ellipsis, yMin=Ellipsis, zMin=Ellipsis, xMax=Ellipsis, yMax=Ellipsis, zMax=Ellipsis)

This method returns an array of element objects that lie within the specified bounding box.

Note

Check MeshElementArray.getByBoundingBox on help.3ds.com/0.1..

Parameters:

• xMin (float, default: Ellipsis) – A float specifying the minimum X boundary of the bounding box.

• yMin (float, default: Ellipsis) – A float specifying the minimum Y boundary of the bounding box.

• zMin (float, default: Ellipsis) – A float specifying the minimum Z boundary of the bounding box.

• xMax (float, default: Ellipsis) – A float specifying the maximum X boundary of the bounding box.

• yMax (float, default: Ellipsis) – A float specifying the maximum Y boundary of the bounding box.

• zMax (float, default: Ellipsis) – A float specifying the maximum Z boundary of the bounding box.

Returns:

A MeshElementArray object, which is a sequence of MeshElement objects.

Return type:

MeshElementArray

getByBoundingCylinder(center1, center2, radius)

This method returns an array of element objects that lie within the specified bounding cylinder.

Note

Check MeshElementArray.getByBoundingCylinder on help.3ds.com/0.1..

Parameters:

• center1 (tuple) – A tuple of the X-, Y-, and Z-coordinates of the center of the first end of the cylinder.

• center2 (tuple) – A tuple of the X-, Y-, and Z-coordinates of the center of the second end of the cylinder.

• radius (str) – A float specifying the radius of the cylinder.

Returns:

A MeshElementArray object, which is a sequence of MeshElement objects.

Return type:

MeshElementArray

getByBoundingSphere(center, radius)

This method returns an array of element objects that lie within the specified bounding sphere.

Note

Check MeshElementArray.getByBoundingSphere on help.3ds.com/0.1..

Parameters:

• center (Tuple[float, float, float]) – A tuple of the X-, Y-, and Z-coordinates of the center of the sphere.

• radius (float) – A float specifying the radius of the sphere.

Returns:

A MeshElementArray object, which is a sequence of MeshElement objects.

Return type:

MeshElementArray

getExteriorEdges()

This method returns the edges on the exterior of the faces in the FaceArray. That is, it returns the edges that are referenced by exactly one of the faces in the sequence.

New in version 2018: The getExteriorEdges method was added.

Returns:

An EdgeArray object specifying the exterior edges.

Return type:

EdgeArray

getExteriorFaces()

This method returns the cell faces on the exterior of the CellArray. That is, it returns the faces that are referenced by exactly one of the cells in the sequence.

New in version 2018: The getExteriorFaces method was added.

Returns:

A FaceArray object representing the faces on the exterior of the cells.

Return type:

FaceArray

getFromLabel(label)

This method returns the object in the MeshElementArray with the given label.

Note

Check MeshElementArray.getFromLabel on help.3ds.com/0.1..

Parameters:

label (int) – An Int specifying the label of the object.

Returns:

A MeshElement object.

Return type:

MeshElement

getMask()

This method returns a string specifying the object or objects.

Returns:

A String specifying the object or objects.

Return type:

str

getSequenceFromMask(mask)

This method returns the objects in the MeshElementArray identified using the specified mask. This command is generated when the JournalOptions are set to COMPRESSEDINDEX. When a large number of objects are involved, this method is highly efficient.

Note

Check MeshElementArray.getSequenceFromMask on help.3ds.com/0.1..

Parameters:

mask (str) – A String specifying the object or objects.

Returns:

A MeshElementArray object.

Return type:

MeshElementArray

sequenceFromLabels(labels)

This method returns the objects in the MeshElementArray identified using the specified labels.

Note

Check MeshElementArray.sequenceFromLabels on help.3ds.com/0.1..

Parameters:

labels (Tuple[int, ...]) – A sequence of Ints specifying the labels.

Returns:

A MeshElementArray object.

Return type:

MeshElementArray

Raises:

Error – An exception occurs if the resulting sequence is empty.

MesherOptions

class MesherOptions

The MesherOptions object controls the default settings that Abaqus uses for all meshing methods. The MesherOptions object has no constructor. Abaqus creates the MesherOptions member when a session is started. MesherOptions commands are intended for use at the beginning of scripts and in the abaqus_v6.env file only; they should not be used during an Abaqus/CAE session.

Note

This object can be accessed by:

session.defaultMesherOptions

Note

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

Public Methods:

setValues([elemShape2D, elemShape3D, ...])

This method modifies the MesherOptions object.

---

setValues(elemShape2D=abaqusConstants.QUAD_DOMINATED, elemShape3D=abaqusConstants.HEX, quadAlgorithm=abaqusConstants.ADVANCING_FRONT, allowMapped=OFF, minTransition=ON, guiPreferredElements=None)

This method modifies the MesherOptions object.

Note

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

Parameters:

• elemShape2D (SymbolicConstant, default: QUAD_DOMINATED) – A SymbolicConstant specifying the default element shape for meshing two-dimensional objects. Possible values are QUAD, QUAD_DOMINATED, and TRI. The default value is QUAD_DOMINATED.

• elemShape3D (SymbolicConstant, default: HEX) – A SymbolicConstant specifying the default element shape for meshing three-dimensional objects. Possible values are HEX, HEX_DOMINATED, WEDGE, and TET. The default value is HEX.

• quadAlgorithm (SymbolicConstant, default: ADVANCING_FRONT) – A SymbolicConstant specifying the default algorithm for meshing an object with quad- or quad-dominated elements. Possible values are ADVANCING_FRONT and MEDIAL_AXIS. The default value is ADVANCING_FRONT.

• allowMapped (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether Abaqus/CAE should allow mapped meshing, where appropriate. The default value is OFF.

• minTransition (Union[AbaqusBoolean, bool], default: ON) – A Boolean specifying whether Abaqus/CAE should attempt to minimize the mesh transition when it moves from a coarse mesh to a fine mesh. The default value is ON.

• guiPreferredElements (Optional[SymbolicConstant], default: None) –

  A list of SymbolicConstants specifying preferred Abaqus element types. This setting is relevant only when Abaqus/CAE is run interactively. When a part or part instance that has never been assigned an element type is meshed, this list is consulted. If an element type appropriate to the geometry is found in the list, it is assigned to the geometry. Multiple element types representing different shapes (for example, triangles and quadrilaterals) can be assigned in combination, but only element types that are compatible with each other are used. When more than one appropriate element type is found in the list, the first element type encountered takes precedence. This list is also consulted when populating the element type dialog; preferred types are selected by default for a region not previously assigned any element types. The default value is an empty list.

  New in version 2018: The guiPreferredElements argument was added.

MeshFace

class MeshFace

The MeshFace object refers to an element face. It has no constructor or members. A MeshFace object can be accessed via a MeshFaceArray or a repository on a part or part instance.

Note

This object can be accessed by:

import part
mdb.models[name].parts[name].elementFaces[i]
mdb.models[name].parts[name].elemFaces[i]
import assembly
mdb.models[name].rootAssembly.allInstances[name].elementFaces[i]
mdb.models[name].rootAssembly.allInstances[name].elemFaces[i]
mdb.models[name].rootAssembly.instances[name].elementFaces[i]
mdb.models[name].rootAssembly.instances[name].elemFaces[i]

Note

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

Public Data Attributes:

label	An Int specifying an Int specifying the element label.
face	An Int specifying a symbolic constant specifying the side of the element.

Public Methods:

getElemEdges()	This method returns a tuple of unique element edges on the element face.
getElements()	This method returns a tuple of elements that share the element face.
getNodes()	This method returns a tuple of nodes on the element face.
getNodesByFaceAngle(angle)	This method returns an array of mesh node objects that are obtained by recursively finding adjacent element faces that are at an angle of less than or equal to the specified angle.
getNormal()	This method returns the normal direction for the element face.
getElemFacesByFaceAngle(angle)	This method returns an array of element face objects that are obtained by recursively finding adjacent element faces that are at an angle of less than or equal to the specified angle.
getElemEdgesByFaceAngle(angle)	This method returns an array of element edge objects that are obtained by recursively finding adjacent element edges that are at an angle of less than or equal to the specified face angle.
getElementsByFaceAngle(angle)	This method returns an array of mesh Element objects that are obtained by recursively finding adjacent element faces that are at an angle of less than or equal to the specified angle.
getElemFacesByLimitingAngle(angle)	This method returns an array of element edge objects that are obtained by recursively finding adjacent element faces that are at an angle of less than or equal to the specified face angle with the seed face.
getElementsViaTopology()	This method returns an array of mesh Element objects that are obtained by recursively finding adjacent elements via topology.
getElemFacesByLayer(numLayers)	This method returns an array of element face objects, obtained by traversing shell elements or the exterior of a solid mesh, and recursively finding adjacent element faces by layer.

---

face: Optional[int] = None

An Int specifying a symbolic constant specifying the side of the element.

getElemEdges()

This method returns a tuple of unique element edges on the element face.

Returns:

edges – A tuple of MeshEdge objects

Return type:

Tuple[MeshEdge, ]

getElemEdgesByFaceAngle(angle)

This method returns an array of element edge objects that are obtained by recursively finding adjacent element edges that are at an angle of less than or equal to the specified face angle.

Note

Check MeshFace.getElemEdgesByFaceAngle on help.3ds.com/0.1..

Parameters:

angle (str) – A float specifying the value of the face angle in degrees.

Returns:

edges – A MeshEdgeArray object, which is a sequence of MeshEdge objects.

Return type:

MeshEdgeArray

getElemFacesByFaceAngle(angle)

This method returns an array of element face objects that are obtained by recursively finding adjacent element faces that are at an angle of less than or equal to the specified angle.

Note

Check MeshFace.getElemFacesByFaceAngle on help.3ds.com/0.1..

Parameters:

angle (str) – A float specifying the value of the face angle.

Returns:

faces – A MeshFaceArray object, which is a sequence of MeshFace objects.

Return type:

MeshFaceArray

getElemFacesByLayer(numLayers)

This method returns an array of element face objects, obtained by traversing shell elements or the exterior of a solid mesh, and recursively finding adjacent element faces by layer.

Note

Check MeshFace.getElemFacesByLayer on help.3ds.com/0.1..

Parameters:

numLayers (str) – A int specifying the value of the number of layers.

Returns:

faces – A MeshFaceArray object, which is a sequence of MeshFace objects.

Return type:

MeshFaceArray

getElemFacesByLimitingAngle(angle)

This method returns an array of element edge objects that are obtained by recursively finding adjacent element faces that are at an angle of less than or equal to the specified face angle with the seed face.

Note

Check MeshFace.getElemFacesByLimitingAngle on help.3ds.com/0.1..

Parameters:

angle (str) – A float specifying the value of the face angle in degrees.

Returns:

faces – A MeshFaceArray object, which is a sequence of MeshFace objects.

Return type:

MeshFaceArray

getElements()

This method returns a tuple of elements that share the element face.

Returns:

elements – A tuple of MeshElement objects

Return type:

Tuple[MeshElement, ]

getElementsByFaceAngle(angle)

This method returns an array of mesh Element objects that are obtained by recursively finding adjacent element faces that are at an angle of less than or equal to the specified angle.

Note

Check MeshFace.getElementsByFaceAngle on help.3ds.com/0.1..

Parameters:

angle (str) – A float specifying the value of the face angle.

Returns:

elements – A MeshElementArray object, which is a sequence of MeshElement objects.

Return type:

MeshElementArray

getElementsViaTopology()

This method returns an array of mesh Element objects that are obtained by recursively finding adjacent elements via topology.

Returns:

elements – A MeshElementArray object, which is a sequence of MeshElement objects.

Return type:

MeshElementArray

getNodes()

This method returns a tuple of nodes on the element face.

Returns:

nodes – A tuple of MeshNode objects

Return type:

Tuple[MeshNode, ]

getNodesByFaceAngle(angle)

This method returns an array of mesh node objects that are obtained by recursively finding adjacent element faces that are at an angle of less than or equal to the specified angle.

Note

Check MeshFace.getNodesByFaceAngle on help.3ds.com/0.1..

Parameters:

angle (str) – A float specifying the value of the face angle.

Returns:

nodes – A MeshNodeArray object, which is a sequence of MeshNode objects

Return type:

MeshNodeArray

getNormal()

This method returns the normal direction for the element face.

Returns:

normal – A tuple of 3 floats representing the unit normal vector. If the element face is collapsed such that a normal cannot be computed, a zero-length vector is returned.

Return type:

Tuple[float, ]

label: Optional[int] = None

An Int specifying an Int specifying the element label.

MeshFaceArray

class MeshFaceArray(elemFaces)

The MeshFaceArray is a sequence of MeshFace objects.

Note

This object can be accessed by:

import part
mdb.models[name].parts[name].elementFaces
import assembly
mdb.models[name].rootAssembly.allInstances[name].elementFaces
mdb.models[name].rootAssembly.instances[name].elementFaces

Note

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

Public Methods:

__init__(elemFaces)	This method creates a MeshFaceArray object.
getSequenceFromMask(mask)	This method returns the objects in the MeshFaceArray identified using the specified mask.
getMask()	This method returns a string specifying the object or objects.

Inherited from list

__repr__()	Return repr(self).
__getattribute__(name, /)	Return getattr(self, name).
__lt__(value, /)	Return self<value.
__le__(value, /)	Return self<=value.
__eq__(value, /)	Return self==value.
__ne__(value, /)	Return self!=value.
__gt__(value, /)	Return self>value.
__ge__(value, /)	Return self>=value.
__iter__()	Implement iter(self).
__init__(elemFaces)	This method creates a MeshFaceArray object.
__len__()	Return len(self).
__getitem__	x.__getitem__(y) <==> x[y]
__setitem__(key, value, /)	Set self[key] to value.
__delitem__(key, /)	Delete self[key].
__add__(value, /)	Return self+value.
__mul__(value, /)	Return self*value.
__rmul__(value, /)	Return value*self.
__contains__(key, /)	Return key in self.
__iadd__(value, /)	Implement self+=value.
__imul__(value, /)	Implement self*=value.
__reversed__()	Return a reverse iterator over the list.
__sizeof__()	Return the size of the list in memory, in bytes.
clear()	Remove all items from list.
copy()	Return a shallow copy of the list.
append(object, /)	Append object to the end of the list.
insert(index, object, /)	Insert object before index.
extend(iterable, /)	Extend list by appending elements from the iterable.
pop([index])	Remove and return item at index (default last).
remove(value, /)	Remove first occurrence of value.
index(value[, start, stop])	Return first index of value.
count(value, /)	Return number of occurrences of value.
reverse()	Reverse IN PLACE.
sort(*[, key, reverse])	Sort the list in ascending order and return None.
__class_getitem__	See PEP 585

Inherited from Generic

__class_getitem__	See PEP 585
__init_subclass__(*args, **kwargs)	This method is called when a class is subclassed.

Private Data Attributes:

Inherited from Generic

_is_protocol

---

getMask()

This method returns a string specifying the object or objects.

Returns:

A String specifying the object or objects.

Return type:

str

getSequenceFromMask(mask)

This method returns the objects in the MeshFaceArray identified using the specified mask. When large number of objects are involved, this method is highly efficient.

Note

Check MeshFaceArray.getSequenceFromMask on help.3ds.com/0.1..

Parameters:

mask (str) – A String specifying the object or objects.

Returns:

A MeshFaceArray object.

Return type:

MeshFaceArray

Raises:

Error – An exception occurs if the resulting sequence is empty.

MeshNode

class MeshNode(coordinates, localCsys=None, label=None)

The MeshNode object refers to a node of a native mesh or an orphan mesh. A MeshNode object can be accessed via a part or part instance using an index that refers to the internal numbering of the node repository. The index does not refer to the node label.

Note

This object can be accessed by:

import part
mdb.models[name].parts[name].allInternalSets[name].nodes[i]
mdb.models[name].parts[name].allInternalSurfaces[name].nodes[i]
mdb.models[name].parts[name].allSets[name].nodes[i]
mdb.models[name].parts[name].allSurfaces[name].nodes[i]
mdb.models[name].parts[name].nodes[i]
mdb.models[name].parts[name].retainedNodes[i]
mdb.models[name].parts[name].sets[name].nodes[i]
mdb.models[name].parts[name].surfaces[name].nodes[i]
import assembly
mdb.models[name].rootAssembly.allInstances[name].nodes[i]
mdb.models[name].rootAssembly.allInstances[name].sets[name].nodes[i]
mdb.models[name].rootAssembly.allInstances[name].surfaces[name].nodes[i]
mdb.models[name].rootAssembly.allInternalSets[name].nodes[i]
mdb.models[name].rootAssembly.allInternalSurfaces[name].nodes[i]
mdb.models[name].rootAssembly.allSets[name].nodes[i]
mdb.models[name].rootAssembly.allSurfaces[name].nodes[i]
mdb.models[name].rootAssembly.instances[name].nodes[i]
mdb.models[name].rootAssembly.instances[name].sets[name].nodes[i]
mdb.models[name].rootAssembly.instances[name].surfaces[name].nodes[i]
mdb.models[name].rootAssembly.modelInstances[i].nodes[i]
mdb.models[name].rootAssembly.modelInstances[i].sets[name].nodes[i]
mdb.models[name].rootAssembly.modelInstances[i].surfaces[name].nodes[i]
mdb.models[name].rootAssembly.nodes[i]
mdb.models[name].rootAssembly.sets[name].nodes[i]
mdb.models[name].rootAssembly.surfaces[name].nodes[i]

Note

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

Public Data Attributes:

label	An Int specifying the node label.
instanceName	A String specifying the name of the part instance that owns this node.
coordinates	A tuple of three Floats specifying the coordinates of the new node.

Public Methods:

__init__(coordinates[, localCsys, label])	This method creates a node on an orphan mesh part.
getElemEdges()	This method returns a tuple of element edge objects that share the node.
getElemFaces()	This method returns a tuple of element face objects that share the node.
getElements()	This method returns a tuple of element objects that share the node.
getNodesByFeatureEdge(angle)	This method returns an array of mesh node objects that are obtained by recursively finding adjacent nodes along a feature edge that are at an angle of less than or equal to the specified face angle.
setValues([label])	This method modifies the MeshNode object.

---

coordinates: Optional[float] = None

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

getElemEdges()

This method returns a tuple of element edge objects that share the node.

Returns:

edges – A tuple of MeshEdge objects

Return type:

Tuple[MeshEdge, ]

getElemFaces()

This method returns a tuple of element face objects that share the node.

Returns:

faces – A tuple of MeshFace objects

Return type:

Tuple[MeshFace, ]

getElements()

This method returns a tuple of element objects that share the node.

Returns:

elements – A tuple of MeshElement objects

Return type:

Tuple[MeshElement, ]

getNodesByFeatureEdge(angle)

This method returns an array of mesh node objects that are obtained by recursively finding adjacent nodes along a feature edge that are at an angle of less than or equal to the specified face angle.

Note

Check MeshNode.getNodesByFeatureEdge on help.3ds.com/0.1..

Parameters:

angle (str) – A float specifying the value of the face angle in degrees.

Returns:

nodes – A MeshNodeArray object, which is a sequence of MeshNode objects

Return type:

MeshNodeArray

instanceName: str = ''

A String specifying the name of the part instance that owns this node.

label: Optional[int] = None

An Int specifying the node label.

setValues(label=None)

This method modifies the MeshNode object.

Note

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

Parameters:

label (Optional[int], default: None) – An Int specifying the node label. This member may only be edited if the node belongs to an orphan mesh part. The specified label must be non-negative and must not be in use by any other node of the same part.

MeshNodeArray

class MeshNodeArray(nodes)

The MeshNodeArray is a sequence of MeshNode objects.

Note

This object can be accessed by:

import part
mdb.models[name].parts[name].allInternalSets[name].nodes
mdb.models[name].parts[name].allInternalSurfaces[name].nodes
mdb.models[name].parts[name].allSets[name].nodes
mdb.models[name].parts[name].allSurfaces[name].nodes
mdb.models[name].parts[name].nodes
mdb.models[name].parts[name].retainedNodes
mdb.models[name].parts[name].sets[name].nodes
mdb.models[name].parts[name].surfaces[name].nodes
import assembly
mdb.models[name].rootAssembly.allInstances[name].nodes
mdb.models[name].rootAssembly.allInstances[name].sets[name].nodes
mdb.models[name].rootAssembly.allInstances[name].surfaces[name].nodes
mdb.models[name].rootAssembly.allInternalSets[name].nodes
mdb.models[name].rootAssembly.allInternalSurfaces[name].nodes
mdb.models[name].rootAssembly.allSets[name].nodes
mdb.models[name].rootAssembly.allSurfaces[name].nodes
mdb.models[name].rootAssembly.instances[name].nodes
mdb.models[name].rootAssembly.instances[name].sets[name].nodes
mdb.models[name].rootAssembly.instances[name].surfaces[name].nodes
mdb.models[name].rootAssembly.modelInstances[i].nodes
mdb.models[name].rootAssembly.modelInstances[i].sets[name].nodes
mdb.models[name].rootAssembly.modelInstances[i].surfaces[name].nodes
mdb.models[name].rootAssembly.nodes
mdb.models[name].rootAssembly.sets[name].nodes
mdb.models[name].rootAssembly.surfaces[name].nodes

Note

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

Public Methods:

__init__(nodes)	This method creates a MeshNodeArray object.
getFromLabel(label)	This method returns the object in the MeshNodeArray with the given label.
getSequenceFromMask(mask)	This method returns the objects in the MeshNodeArray identified using the specified mask.
getMask()	This method returns a string specifying the object or objects.
getByBoundingBox([xMin, yMin, zMin, xMax, ...])	This method returns an array of nodes that lie within the specified bounding box.
getByBoundingCylinder(center1, center2, radius)	This method returns an array of node objects that lie within the specified bounding cylinder.
getByBoundingSphere(center, radius)	This method returns an array of node objects that lie within the specified bounding sphere.
getBoundingBox()	This method returns a dictionary of two tuples representing minimum and maximum boundary values of the bounding box of the minimum size containing the node sequence.
getClosest(coordinates[, numToFind, ...])	This method returns the node or nodes closest to the given point or set of points.
sequenceFromLabels(labels)	This method returns the objects in the MeshNodeArray identified using the specified labels.

Inherited from list

__repr__()	Return repr(self).
__getattribute__(name, /)	Return getattr(self, name).
__lt__(value, /)	Return self<value.
__le__(value, /)	Return self<=value.
__eq__(value, /)	Return self==value.
__ne__(value, /)	Return self!=value.
__gt__(value, /)	Return self>value.
__ge__(value, /)	Return self>=value.
__iter__()	Implement iter(self).
__init__(nodes)	This method creates a MeshNodeArray object.
__len__()	Return len(self).
__getitem__	x.__getitem__(y) <==> x[y]
__setitem__(key, value, /)	Set self[key] to value.
__delitem__(key, /)	Delete self[key].
__add__(value, /)	Return self+value.
__mul__(value, /)	Return self*value.
__rmul__(value, /)	Return value*self.
__contains__(key, /)	Return key in self.
__iadd__(value, /)	Implement self+=value.
__imul__(value, /)	Implement self*=value.
__reversed__()	Return a reverse iterator over the list.
__sizeof__()	Return the size of the list in memory, in bytes.
clear()	Remove all items from list.
copy()	Return a shallow copy of the list.
append(object, /)	Append object to the end of the list.
insert(index, object, /)	Insert object before index.
extend(iterable, /)	Extend list by appending elements from the iterable.
pop([index])	Remove and return item at index (default last).
remove(value, /)	Remove first occurrence of value.
index(value[, start, stop])	Return first index of value.
count(value, /)	Return number of occurrences of value.
reverse()	Reverse IN PLACE.
sort(*[, key, reverse])	Sort the list in ascending order and return None.
__class_getitem__	See PEP 585

Inherited from Generic

__class_getitem__	See PEP 585
__init_subclass__(*args, **kwargs)	This method is called when a class is subclassed.

Private Data Attributes:

Inherited from Generic

_is_protocol

---

getBoundingBox()

This method returns a dictionary of two tuples representing minimum and maximum boundary values of the bounding box of the minimum size containing the node sequence.

Returns:

A Dictionary object with the following items:

• low: a tuple of three floats representing the minimum x, y and z boundary values of the bounding box.

• high: a tuple of three floats representing the maximum x, y and z boundary values of the bounding box.

Return type:

Dict[str, Tuple[float, float, float]]

getByBoundingBox(xMin=Ellipsis, yMin=Ellipsis, zMin=Ellipsis, xMax=Ellipsis, yMax=Ellipsis, zMax=Ellipsis)

This method returns an array of nodes that lie within the specified bounding box.

Note

Check MeshNodeArray.getByBoundingBox on help.3ds.com/0.1..

Parameters:

• xMin (float, default: Ellipsis) – A float specifying the minimum X boundary of the bounding box.

• yMin (float, default: Ellipsis) – A float specifying the minimum Y boundary of the bounding box.

• zMin (float, default: Ellipsis) – A float specifying the minimum Z boundary of the bounding box.

• xMax (float, default: Ellipsis) – A float specifying the maximum X boundary of the bounding box.

• yMax (float, default: Ellipsis) – A float specifying the maximum Y boundary of the bounding box.

• zMax (float, default: Ellipsis) – A float specifying the maximum Z boundary of the bounding box.

Returns:

A MeshNodeArray object, which is a sequence of MeshNode objects.

Return type:

MeshNodeArray

getByBoundingCylinder(center1, center2, radius)

This method returns an array of node objects that lie within the specified bounding cylinder.

Note

Check MeshNodeArray.getByBoundingCylinder on help.3ds.com/0.1..

Parameters:

• center1 (Tuple[float, float, float]) – A tuple of the X-, Y-, and Z-coordinates of the center of the first end of the cylinder.

• center2 (Tuple[float, float, float]) – A tuple of the X-, Y-, and Z-coordinates of the center of the second end of the cylinder.

• radius (float) – A float specifying the radius of the cylinder.

Returns:

A MeshNodeArray object, which is a sequence of MeshNode objects.

Return type:

MeshNodeArray

getByBoundingSphere(center, radius)

This method returns an array of node objects that lie within the specified bounding sphere.

Note

Check MeshNodeArray.getByBoundingSphere on help.3ds.com/0.1..

Parameters:

• center (tuple) – A tuple of the X-, Y-, and Z-coordinates of the center of the sphere.

• radius (str) – A float specifying the radius of the sphere.

Returns:

A MeshNodeArray object, which is a sequence of MeshNode objects.

Return type:

MeshNodeArray

getClosest(coordinates, numToFind=1, searchTolerance=Ellipsis)

This method returns the node or nodes closest to the given point or set of points.

Note

Check MeshNodeArray.getClosest on help.3ds.com/0.1..

Parameters:

• coordinates (str) – A point defined by x, y, and z values or a list of such points.

• numToFind (int, default: 1) – The number of nodes to find for each given point. For example, if numToFind is 2, then the 2 closest points, if available and within searchTolerance, will be returned in order of proximity for each input point. The default is 1.

• searchTolerance (float, default: Ellipsis) – A float specifying a search radius for each point. By default, no search radius is defined, and all nodes in the sequence will be searched.

Returns:

A MeshNode, or a list of MeshNode objects, or a list of lists of MeshNode objects, depending on the number of points given and the number of nodes requested.

Return type:

MeshNode | List[MeshNode]

getFromLabel(label)

This method returns the object in the MeshNodeArray with the given label.

Note

Check MeshNodeArray.getFromLabel on help.3ds.com/0.1..

Parameters:

label (int) – An Int specifying the label of the object.

Returns:

A MeshNode object.

Return type:

MeshNode

getMask()

This method returns a string specifying the object or objects.

Returns:

A String specifying the object or objects.

Return type:

str

getSequenceFromMask(mask)

This method returns the objects in the MeshNodeArray identified using the specified mask. This command is generated when the JournalOptions are set to COMPRESSEDINDEX. When a large number of objects are involved, this method is highly efficient.

Note

Check MeshNodeArray.getSequenceFromMask on help.3ds.com/0.1..

Parameters:

mask (str) – A String specifying the object or objects.

Returns:

A MeshNodeArray object.

Return type:

MeshNodeArray

sequenceFromLabels(labels)

This method returns the objects in the MeshNodeArray identified using the specified labels.

Note

Check MeshNodeArray.sequenceFromLabels on help.3ds.com/0.1..

Parameters:

labels (Tuple[int, ...]) – A sequence of Ints specifying the labels.

Returns:

A MeshNodeArray object.

Return type:

MeshNodeArray

Raises:

Error – An exception occurs if the resulting sequence is empty.

MeshPart

class MeshPart(name: str, dimensionality: SymbolicConstant, type: SymbolicConstant, twist: Union[AbaqusBoolean, bool] = OFF)

class MeshPart(name: str, objectToCopy: str, scale: float = 1, mirrorPlane: SymbolicConstant = NONE, compressFeatureList: Union[AbaqusBoolean, bool] = OFF, separate: Union[AbaqusBoolean, bool] = OFF)

The following commands operate on Part objects. For more information about the Part object, see Part object.

Note

This object can be accessed by:

import mesh

Note

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

Public Data Attributes:

Inherited from PartBase

geometryValidity	A Boolean specifying the validity of the geometry of the part.
isOutOfDate	An Int specifying that feature parameters have been modified but that the part has not been regenerated.
timeStamp	A Float specifying when the part was last modified.
vertices	A VertexArray object specifying all the vertices in the part.
ignoredVertices	An IgnoredVertexArray object specifying all the ignored vertices in the part.
edges	An EdgeArray object specifying all the edges in the part.
ignoredEdges	An IgnoredEdgeArray object specifying all the ignored edges in the part.
faces	A FaceArray object specifying all the faces in the part.
cells	A CellArray object specifying all the cells in the part.
features	A repository of Feature objects specifying all the features in the part.
featuresById	A repository of Feature objects specifying all Feature objects in the part.
datums	A repository of Datum objects specifying all the datums in the part.
elements	A MeshElementArray object specifying all the elements in the part.
elemFaces	A repository of MeshFace objects specifying all the element faces in the part.
elementFaces	A MeshFaceArray object specifying all the unique element faces in the part.
nodes	A MeshNodeArray object specifying all the nodes in the part.
retainedNodes	A MeshNodeArray object specifying all the retained nodes in the substructure part.
sets	A repository of Set objects specifying for more information, see Set.
allSets	A repository of Set objects specifying the contents of the allSets repository is the same as the contents of the sets repository.
allInternalSets	A repository of Set objects specifying picked regions.
surfaces	A repository of Surface objects specifying for more information, see Surface.
allSurfaces	A repository of Surface objects specifying the contents of the allSurfaces repository is the same as the contents of the surfaces repository.
allInternalSurfaces	A repository of Surface objects specifying picked regions.
skins	A repository of Skin objects specifying the skins created on the part.
stringers	A repository of Stringer objects specifying the stringers created on the part.
referencePoints	A repository of ReferencePoint objects.
engineeringFeatures	An EngineeringFeature object.
sectionAssignments	A SectionAssignmentArray object.
materialOrientations	A MaterialOrientationArray object.
compositeLayups	A repository of CompositeLayup objects.
elemEdges	A repository of MeshEdge objects specifying all the element edges in the part.
elementEdges	A MeshEdgeArray object specifying all the unique element edges in the part.

Inherited from Feature

name	A String specifying the repository key.
id	An Int specifying the ID of the feature.

Public Methods:

assignStackDirection(cells, referenceRegion)	This method assigns a stack direction to geometric cells.
associateMeshWithGeometry(geometricEntity[, ...])	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.
createVirtualTopology([regions, ...])	This method creates a virtual topology feature by automatically merging faces and edges based on a set of geometric parameters.
deleteBoundaryLayerControls(regions)	This method deletes the control parameters for boundary layer mesh for all the specified regions.
deleteMesh(regions)	This method deletes a subset of the mesh that contains the native elements from the given parts or regions.
deleteMeshAssociationWithGeometry(...[, ...])	This method deletes the association of geometric entities with mesh entities.
deletePreviewMesh()	This method deletes all boundary meshes in the parts.
deleteSeeds(regions)	This method deletes the global edge seeds from the given parts or deletes the local edge seeds from the given edges.
generateMesh([regions, ...])	This method generates a mesh in the given parts or regions.
generateBottomUpExtrudedMesh(cell, ...[, ...])	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.
generateBottomUpSweptMesh(cell[, ...])	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.
generateBottomUpRevolvedMesh(cell, ...[, ...])	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.
getEdgeSeeds(edge, attribute)	This method returns an edge seed parameter for a specified edge of a part.
getElementType(region, elemShape)	This method returns the ElemType object of a given element shape assigned to a region of a part.
getIncompatibleMeshInterfaces([cells])	This method returns a sequence of Face objects that are meshed with incompatible elements.
getMeshControl(region, attribute)	This method returns a mesh control parameter for the specified region of a part.
getMeshStats(regions)	This method returns the mesh statistics for the given regions.
getPartSeeds(attribute)	This method returns a part seed parameter for the part.
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.
ignoreEntity(entities)	This method creates a virtual topology feature.
restoreIgnoredEntity(entities)	This method restores vertices and edges that have been merged using a virtual topology feature.
seedEdgeByBias(biasMethod, end1Edges, ...[, ...])	This method seeds the given edges nonuniformly using the specified number of elements and bias ratio or the specified minimum and maximum element sizes.
seedEdgeByNumber(edges, number[, constraint])	This method seeds the given edges uniformly based on the number of elements along the edges.
seedEdgeBySize(edges, size[, ...])	This method seeds the given edges either uniformly or following edge curvature distribution, based on the desired element size.
seedPart(size[, deviationFactor, ...])	This method assigns global edge seeds to the given parts.
setBoundaryLayerControls(regions, ...[, ...])	This method sets the control parameters for boundary layer mesh for the specified regions.
setElementType(regions, elemTypes)	This method assigns element types to the specified regions.
setLogicalCorners(region, corners)	This method sets the logical corners for a mappable face region.
setMeshControls(regions[, elemShape, ...])	This method sets the mesh control parameters for the specified regions.
setSweepPath(region, edge, sense)	This method sets the sweep path for a sweepable region or the revolve path for a revolvable region.
verifyMeshQuality(criterion[, threshold, ...])	This method tests the mesh quality of a part and returns poor-quality elements.
Node(coordinates[, localCsys, label])	This method creates a node on an orphan mesh part.

Inherited from PartBase

__init__(*args, **kwargs)
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.
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.
setValues(*args, **kwargs)	This method modifies the Part object.
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.
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])	Location of the centroid of a given face/cell or group of faces/cells
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:
getLength(edges)	This method returns the length of a given edge or group of edges.
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.
getMassProperties([regions, ...])	This method returns the mass properties of a part or region.
getFeatureFaces(name)	This method returns a sequence of Face 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.
getFeatureCells(name)	This method returns a sequence of Cell 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.
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.
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.
queryDisjointPlyRegions()	This method provides a list of all composite plys in the current part which have disjoint regions.
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.
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.
copyMeshPattern(elements, faces, elemFaces, ...)	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.
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
Lock()	This method locks the part.
Unlock()	This method unlocks the part.
LockForUpgrade()	This method locks the part for upgrade.

Inherited from PartFeature

AutoRepair()	This method carries out a sequence of geometry repair operations if it contains invalid entities.
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.
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.
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.
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.
Mirror(mirrorPlane, keepOriginal[, ...])	This method mirrors existing part geometry across a plane to create new geometry.
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.
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.
WireSpline(points[, mergeType, ...])	This method creates an additional Feature object by creating a spline wire that passes through a sequence of given points.
WirePolyLine(points[, mergeType, meshable])	This method creates an additional Feature object by creating a polyline wire that passes through a sequence of given points.
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.

Inherited from Feature

AttachmentPoints(name, points[, ...])	This method creates an attachment points Feature.
AttachmentPointsAlongDirection(name, ...[, ...])	This method creates a Feature object by creating attachment points along a direction or between two points.
AttachmentPointsOffsetFromEdges(name, edges)	This method creates a Feature object by creating attachment points along or offset from one or more connected edges.
DatumAxisByCylFace(face)	This method creates a Feature object and a DatumAxis object along the axis of a cylinder or cone.
DatumAxisByNormalToPlane(plane, point)	This method creates a Feature object and a DatumAxis object normal to the specified plane and passing through the specified point.
DatumAxisByParToEdge(edge, point)	This method creates a Feature object and a DatumAxis object parallel to the specified edge and passing through the specified point.
DatumAxisByPrincipalAxis(principalAxis)	This method creates a Feature object and a DatumAxis object along one of the three principal axes.
DatumAxisByRotation(*args, **kwargs)
DatumAxisByThreePoint(point1, point2, point3)	This method creates a Feature object and a DatumAxis object normal to the circle described by three points and through its center.
DatumAxisByThruEdge(edge)	This method creates a Feature object and a DatumAxis object along the specified edge.
DatumAxisByTwoPlane(plane1, plane2)	This method creates a Feature object and a DatumAxis object at the intersection of two planes.
DatumAxisByTwoPoint(point1, point2)	This method creates a Feature object and a DatumAxis object along the line joining two points.
DatumCsysByDefault(coordSysType[, name])	This method creates a Feature object and a DatumCsys object from the specified default coordinate system at the origin.
DatumCsysByOffset(coordSysType, ...[, name])	This method creates a Feature object and a DatumCsys object by offsetting the origin of an existing datum coordinate system to a specified point.
DatumCsysByThreePoints(coordSysType, origin, ...)	This method creates a Feature object and a DatumCsys object from three points.
DatumCsysByTwoLines(coordSysType, line1, line2)	This method creates a Feature object and a DatumCsys object from two orthogonal lines.
DatumPlaneByPrincipalPlane(principalPlane, ...)	This method creates a Feature object and a DatumPlane object through the origin along one of the three principal planes.
DatumPlaneByOffset(*args, **kwargs)
DatumPlaneByRotation(plane, axis, angle)	This method creates a Feature object and a DatumPlane object by rotating a plane about the specified axis through the specified angle.
DatumPlaneByThreePoints(point1, point2, point3)	This method creates a Feature object and a DatumPlane object defined by passing through three points.
DatumPlaneByLinePoint(line, point)	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.
DatumPlaneByPointNormal(point, normal)	This method creates a Feature object and a DatumPlane object normal to the specified line and running through the specified point.
DatumPlaneByTwoPoint(point1, point2)	This method creates a Feature object and a DatumPlane object midway between two points and normal to the line connecting the points.
DatumPointByCoordinate(coords)	This method creates a Feature object and a DatumPoint object at the point defined by the specified coordinates.
DatumPointByOffset(point, vector)	This method creates a Feature object and a DatumPoint object offset from an existing point by a vector.
DatumPointByMidPoint(point1, point2)	This method creates a Feature object and a DatumPoint object midway between two points.
DatumPointByOnFace(face, edge1, offset1, ...)	This method creates a Feature object and a DatumPoint object on the specified face, offset from two edges.
DatumPointByEdgeParam(edge, parameter)	This method creates a Feature object and a DatumPoint object along an edge at a selected distance from one end of the edge.
DatumPointByProjOnEdge(point, edge)	This method creates a Feature object and a DatumPoint object along an edge by projecting an existing point along the normal to the edge.
DatumPointByProjOnFace(point, face)	This method creates a Feature object and a DatumPoint object on a specified face by projecting an existing point onto the face.
MakeSketchTransform(sketchPlane[, origin, ...])	This method creates a Transform object.
PartitionCellByDatumPlane(cells, datumPlane)	This method partitions one or more cells using the given datum plane.
PartitionCellByExtendFace(cells, extendFace)	This method partitions one or more cells by extending the underlying geometry of a given face to partition the target cells.
PartitionCellByExtrudeEdge(cells, edges, ...)	This method partitions one or more cells by extruding selected edges in the given direction.
PartitionCellByPatchNCorners(cell, cornerPoints)	This method partitions a cell using an N-sided cutting patch defined by the given corner points.
PartitionCellByPatchNEdges(cell, edges)	This method partitions a cell using an N-sided cutting patch defined by the given edges.
PartitionCellByPlaneNormalToEdge(cells, ...)	This method partitions one or more cells using a plane normal to an edge at the given edge point.
PartitionCellByPlanePointNormal(cells, ...)	This method partitions one or more cells using a plane defined by a point and a normal direction.
PartitionCellByPlaneThreePoints(cells, ...)	This method partitions one or more cells using a plane defined by three points.
PartitionCellBySweepEdge(cells, edges, sweepPath)	This method partitions one or more cells by sweeping selected edges along the given sweep path.
PartitionEdgeByDatumPlane(edges, datumPlane)	This method partitions an edge where it intersects with a datum plane.
PartitionEdgeByParam(edges, parameter)	This method partitions one or more edges at the given normalized edge parameter.
PartitionEdgeByPoint(edge, point)	This method partitions an edge at the given point.
PartitionFaceByAuto(face)	This method automatically partitions a target face into simple regions that can be meshed using a structured meshing technique.
PartitionFaceByCurvedPathEdgeParams(face, ...)	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.
PartitionFaceByCurvedPathEdgePoints(face, ...)	This method partitions a face normal to two edges, using a curved path between the two given edge points.
PartitionFaceByDatumPlane(faces, datumPlane)	This method partitions one or more faces using the given datum plane.
PartitionFaceByExtendFace(faces, extendFace)	This method partitions one or more faces by extending the underlying geometry of another given face to partition the target faces.
PartitionFaceByIntersectFace(faces, cuttingFaces)	This method partitions one or more faces using the given cutting faces to partition the target faces.
PartitionFaceByProjectingEdges(faces, edges)	This method partitions one or more faces by projecting the given edges on the target faces.
PartitionFaceByShortestPath(faces, point1, ...)	This method partitions one or more faces using a minimum distance path between the two given points.
PartitionFaceBySketch(faces, sketch[, ...])	This method partitions one or more planar faces by sketching on them.
PartitionFaceBySketchDistance(faces, ...[, ...])	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.
PartitionFaceBySketchRefPoint(faces, ...[, ...])	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.
PartitionFaceBySketchThruAll(faces, ...[, ...])	This method partitions one or more faces by sketching on a sketch plane and then projecting toward the target faces through an infinite distance.
ReferencePoint(point[, instanceName])	This method creates a Feature object and a ReferencePoint object at the specified location.
RemoveWireEdges(wireEdgeList)	This method removes wire edges.
WirePolyLine(points[, mergeType, meshable])	This method creates an additional Feature object by creating a polyline wire that passes through a sequence of given points.
isSuppressed()	This method queries the suppressed state of the feature.
restore()	This method restores the parameters of all features in the assembly to the value they had before a failed regeneration.
resume()	This method resumes suppressed features.
setValues(*args, **kwargs)	This method modifies the Part object.
suppress()	This method suppresses features.

---

Node(coordinates, localCsys=None, label=None)

This method creates a node on an orphan mesh part.

Note

This function can be accessed by:

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

Note

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

Parameters:

• coordinates (tuple) – A sequence of three Floats specifying the coordinates of the new node.

• localCsys (Optional[DatumCsys], default: None) – A DatumCsys object specifying the local coordinate system. If unspecified, the global coordinate system will be used.

• label (Optional[int], default: None) – An Int specifying the node label.

Returns:

A MeshNode object.

Return type:

MeshNode

assignStackDirection(cells, referenceRegion)

This method assigns a stack direction to geometric cells. The stack direction will be used to orient the elements during mesh generation.

Note

Check MeshPart.assignStackDirection on help.3ds.com/0.1..

Parameters:

• cells (Tuple[Cell, ...]) – A sequence of Cell objects specifying regions where to assign the stack direction.

• referenceRegion (Face) – A Face object specifying the top side of the stack direction.

associateMeshWithGeometry(geometricEntity, elements=(), elemFaces=(), elemEdges=(), node=<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.

Note

Check MeshPart.associateMeshWithGeometry on help.3ds.com/0.1..

Parameters:

• geometricEntity (str) – 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 (Tuple[MeshElement, ...], default: ()) – A sequence of MeshElement objects specifying the elements to be associated with the geometric cell.

• elemFaces (Tuple[MeshFace, ...], default: ()) – A sequence of Mesh:py:class:~abaqus.BasicGeometry.Face.Face objects specifying the element faces to be associated with the geometric face.

• elemEdges (Tuple[MeshEdge, ...], default: ()) – A sequence of MeshEdge objects specifying the element edges to be associated with the geometric edge.

• node (MeshNode, default: <abaqus.Mesh.MeshNode.MeshNode object at 0x7f350e3436d0>) – A MeshNode object specifying the mesh node to be associated with the geometric vertex.

createVirtualTopology(regions=(), mergeShortEdges=False, shortEdgeThreshold=None, mergeSmallFaces=False, smallFaceAreaThreshold=None, mergeSliverFaces=False, faceAspectRatioThreshold=None, mergeSmallAngleFaces=False, smallFaceCornerAngleThreshold=None, mergeThinStairFaces=False, thinStairFaceThreshold=None, ignoreRedundantEntities=False, cornerAngleTolerance=30, applyBlendControls=False, blendSubtendedAngleTolerance=None, blendRadiusTolerance=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.

Note

Check MeshPart.createVirtualTopology on help.3ds.com/0.1..

Parameters:

• regions (Tuple[Face, ...], default: ()) – 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 (Union[AbaqusBoolean, bool], default: False) – A Boolean specifying whether to merge short edges. The default value is False.

• shortEdgeThreshold (Optional[float], default: None) – 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 (Union[AbaqusBoolean, bool], default: False) – A Boolean specifying whether to merge faces with small area. The default value is False.

• smallFaceAreaThreshold (Optional[float], default: None) – 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 (Union[AbaqusBoolean, bool], default: False) – A Boolean specifying whether to merge faces with high aspect ratio. The default value is False.

• faceAspectRatioThreshold (Optional[float], default: None) – 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 (Union[AbaqusBoolean, bool], default: False) – A Boolean specifying whether to merge faces that have a sharp corner angle. The default value is False.

• smallFaceCornerAngleThreshold (Optional[float], default: None) – 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 (Union[AbaqusBoolean, bool], default: False) – A Boolean specifying whether to merge faces that represent a thin stair-like feature. The default value is False.

• thinStairFaceThreshold (Optional[float], default: None) – 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 (Union[AbaqusBoolean, bool], default: False) – A Boolean specifying whether to abstract away redundant edges and vertices. The default value is False.

• cornerAngleTolerance (float, default: 30) – 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 (Union[AbaqusBoolean, bool], default: False) – 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 (Optional[float], default: None) – 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 (Optional[float], default: None) – 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 – A Feature object

Return type:

Feature

deleteBoundaryLayerControls(regions)

This method deletes the control parameters for boundary layer mesh for all the specified regions.

Note

Check MeshPart.deleteBoundaryLayerControls on help.3ds.com/0.1..

Parameters:

regions (Tuple[Cell, ...]) – A sequence of Cell objects specifying the regions for which to set the boundary layer mesh control parameters.

deleteMesh(regions)

This method deletes a subset of the mesh that contains the native elements from the given parts or regions.

Note

Check MeshPart.deleteMesh on help.3ds.com/0.1..

Parameters:

regions (Tuple[MeshPart]) – A sequence of Part objects or Region objects specifying the parts or regions from which the native mesh is to be deleted.

deleteMeshAssociationWithGeometry(geometricEntities, addBoundingEntities=False)

This method deletes the association of geometric entities with mesh entities.

Note

Check MeshPart.deleteMeshAssociationWithGeometry on help.3ds.com/0.1..

Parameters:

• geometricEntities (Tuple[Cell, ...]) – A sequence of Cell objects, Face objects, Edge objects, or ConstrainedSketchVertex objects specifying the geometric entities that will be disassociated from the mesh.

• addBoundingEntities (Union[AbaqusBoolean, bool], default: False) – 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.

deletePreviewMesh()

This method deletes all boundary meshes in the parts. See the boundaryPreview argument of generateMesh for information about generating boundary meshes.

deleteSeeds(regions)

This method deletes the global edge seeds from the given parts or deletes the local edge seeds from the given edges.

Note

Check MeshPart.deleteSeeds on help.3ds.com/0.1..

Parameters:

regions (Tuple[MeshPart]) – A sequence of Part objects or Edge objects specifying the parts or edges from which the seeds are to be deleted.

generateBottomUpExtrudedMesh(cell, numberOfLayers, extrudeVector, geometrySourceSide='', elemFacesSourceSide=(), elemSourceSide=(), depth=None, targetSide='', biasRatio=1, extendElementSets=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.

Note

Check MeshPart.generateBottomUpExtrudedMesh on help.3ds.com/0.1..

Parameters:

• cell (Cell) – A Cell object specifying the geometric region where the mesh is to be generated. This argument is valid only for native parts.

• numberOfLayers (int) – An Int specifying the number of layers to be generated along the extrusion vector.

• extrudeVector (tuple) – 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 (str, default: '') – A Region of Face objects specifying the geometric domain to be used as the source for the extrude meshing operation.

• elemFacesSourceSide (Tuple[MeshFace, ...], default: ()) – A sequence of Mesh:py:class:~abaqus.BasicGeometry.Face.Face objects specifying the faces of 3D elements to be used as the source for the extrude meshing operation.

• elemSourceSide (tuple, default: ()) – A sequence of 2D MeshElement objects specifying the elements to be used as the source for the extrude meshing operation.

• depth (Optional[float], default: None) – A Float specifying the distance of the mesh extrusion. If unspecified, the vector length of the extrudeVector argument is assumed.

• targetSide (str, default: '') – A datum plane, a sequence of Face objects, a sequence of Mesh:py:class:~abaqus.BasicGeometry.Face.Face 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 (float, default: 1) – 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 (Union[AbaqusBoolean, bool], default: False) – 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, numberOfLayers, axisOfRevolution, angleOfRevolution, geometrySourceSide='', elemFacesSourceSide=(), elemSourceSide=(), extendElementSets=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.

Note

Check MeshPart.generateBottomUpRevolvedMesh on help.3ds.com/0.1..

Parameters:

• cell (Cell) – A Cell object specifying the geometric region where the mesh is to be generated. This argument is valid only for native parts.

• numberOfLayers (int) – An Int specifying the number of layers of elements to be generated around the axis of revolution.

• axisOfRevolution (tuple) – 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 (float) – A Float specifying the angle of revolution.

• geometrySourceSide (str, default: '') – A Region of Face objects specifying the geometric domain to be used as the source for the revolve meshing operation.

• elemFacesSourceSide (Tuple[MeshFace, ...], default: ()) – A sequence of Mesh:py:class:~abaqus.BasicGeometry.Face.Face objects specifying the faces of 3D elements to be used as the source for the revolve meshing operation.

• elemSourceSide (tuple, default: ()) – A sequence of 2D MeshElement objects specifying the elements to be used as the source for the revolve meshing operation.

• extendElementSets (Union[AbaqusBoolean, bool], default: False) – 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, geometrySourceSide='', elemFacesSourceSide=(), elemSourceSide=(), geometryConnectingSides='', elemFacesConnectingSides=(), elemConnectingSides=(), targetSide=None, numberOfLayers=None, extendElementSets=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.

Note

Check MeshPart.generateBottomUpSweptMesh on help.3ds.com/0.1..

Parameters:

• cell (Cell) – A Cell object specifying the geometric region where the mesh is to be generated. This argument is valid only for native parts.

• geometrySourceSide (str, default: '') – A Region of Face objects specifying the geometric domain to be used as the source for the sweep meshing operation.

• elemFacesSourceSide (Tuple[MeshFace, ...], default: ()) – A sequence of Mesh:py:class:~abaqus.BasicGeometry.Face.Face objects specifying the faces of 3D elements to be used as the source for the sweep meshing operation.

• elemSourceSide (tuple, default: ()) – A sequence of 2D MeshElement objects specifying the elements to be used as the source for the sweep meshing operation.

• geometryConnectingSides (str, default: '') – A Region of Face objects specifying connecting sides of the sweep meshing operation.

• elemFacesConnectingSides (Tuple[MeshFace, ...], default: ()) – A sequence of Mesh:py:class:~abaqus.BasicGeometry.Face.Face objects specifying connecting sides of the sweep meshing operation.

• elemConnectingSides (tuple, default: ()) – A sequence of 2D MeshElement objects specifying connecting sides of the sweep meshing operation.

• targetSide (Optional[Face], default: None) – A Face object specifying the target side of the sweep meshing operation.

• numberOfLayers (Optional[int], default: None) – An Int specifying the number of layers to be generated along the sweep direction.

• extendElementSets (Union[AbaqusBoolean, bool], default: False) – 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(regions=(), seedConstraintOverride=OFF, meshTechniqueOverride=OFF, boundaryPreview=OFF, boundaryMeshOverride=OFF)

This method generates a mesh in the given parts or regions.

Note

Check MeshPart.generateMesh on help.3ds.com/0.1..

Parameters:

• regions (Tuple[MeshPart], default: ()) – A sequence of Part objects or Region objects specifying the parts or regions where the mesh is to be generated.

• seedConstraintOverride (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether mesh generation is allowed to modify seed constraints. The default value is OFF.

• meshTechniqueOverride (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether mesh generation is allowed to modify the existing mesh techniques so that a compatible mesh can be generated. The default value is OFF.

• boundaryPreview (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether the generated mesh should be a boundary preview mesh. This option will only have an effect if any of the specified regions are to be meshed with tetrahedral elements or using the bottom-up technique with hexahedral or wedge elements. The default value is OFF.

• boundaryMeshOverride (Union[AbaqusBoolean, bool], default: OFF) – A Boolean specifying whether mesh generation is allowed to modify an existing boundary preview mesh. This option will only have an effect if any of the specified regions are to be meshed with tetrahedral elements and a boundary preview mesh already exists. The default value is OFF.

getEdgeSeeds(edge, attribute)

This method returns an edge seed parameter for a specified edge of a part.

Note

Check MeshPart.getEdgeSeeds on help.3ds.com/0.1..

Parameters:

• edge (Edge) – An Edge object specifying the edge to be queried.

• attribute (Union[SymbolicConstant, float]) –

  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

Returns:

The return value is a Float, an Int, or a SymbolicConstant depending on the value of the attribute argument.

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.

Return type:

Union[float, int, SymbolicConstant]

getElementType(region, elemShape)

This method returns the ElemType object of a given element shape assigned to a region of a part.

Note

Check MeshPart.getElementType on help.3ds.com/0.1..

Parameters:

• region (str) – A Cell, a Face, or an Edge object specifying the region to be queried.

• elemShape (SymbolicConstant) –

  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:

An ElemType object.

Return type:

ElementType

Raises:

TypeError – The region cannot be associated with element types or the elemShape is not consistent with the dimension of the region.

getIncompatibleMeshInterfaces(cells=())

This method returns a sequence of Face objects that are meshed with incompatible elements.

Note

Check MeshPart.getIncompatibleMeshInterfaces on help.3ds.com/0.1..

Parameters:

cells (Tuple[Cell, ...], default: ()) – A sequence of cell objects which will be used to search the incompatible faces.

Returns:

A sequence of Face objects.

Return type:

Tuple[Face, ]

getMeshControl(region, attribute)

This method returns a mesh control parameter for the specified region of a part.

Note

Check MeshPart.getMeshControl on help.3ds.com/0.1..

Parameters:

• region (str) – A Cell, a Face, or an Edge object specifying the region to be queried.

• attribute (SymbolicConstant) –

  A SymbolicConstant specifying the mesh control attribute to return. Possible values are:

  • ELEM_SHAPE

  • TECHNIQUE

  • ALGORITHM

  • MIN_TRANSITION

  The return value is dependent on 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.

Return type:

Union[bool, SymbolicConstant]

Raises:

TypeError – The region cannot carry mesh controls.

getMeshStats(regions)

This method returns the mesh statistics for the given regions.

Note

Check MeshPart.getMeshStats on help.3ds.com/0.1..

Parameters:

regions (tuple) – A sequence or tuple of ConstrainedSketchGeometry regions for which mesh statistics should be returned.

Returns:

A MeshStats object.

Return type:

MeshStats

getPartSeeds(attribute)

This method returns a part seed parameter for the part.

Note

Check MeshPart.getPartSeeds on help.3ds.com/0.1..

Parameters:

attribute (Union[SymbolicConstant, float]) –

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.

Return type:

float

Raises:

Error – An exception occurs if the part does not contain native geometry.

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.

Return type:

Region

ignoreEntity(entities)

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.

Note

Check MeshPart.ignoreEntity on help.3ds.com/0.1..

Parameters:

entities (tuple) – A sequence of vertices and edges specifying the entities to be ignored during meshing.

Returns:

feature – A Feature object

Return type:

Feature

restoreIgnoredEntity(entities)

This method restores vertices and edges that have been merged using a virtual topology feature.

Note

Check MeshPart.restoreIgnoredEntity on help.3ds.com/0.1..

Parameters:

entities (Tuple[IgnoredVertex, ...]) – A sequence of IgnoredVertex objects and IgnoredEdge objects specifying the entities to be restored.

Returns:

feature – A Feature object

Return type:

Feature

seedEdgeByBias(biasMethod, end1Edges, end2Edges, centerEdges, endEdges, ratio, number, minSize, maxSize, constraint=abaqusConstants.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.

Note

Check MeshPart.seedEdgeByBias on help.3ds.com/0.1..

Parameters:

• biasMethod (SymbolicConstant) – 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 (Tuple[Edge, ...]) – 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 (Tuple[Edge, ...]) – 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 (Tuple[Edge, ...]) – 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 (Tuple[Edge, ...]) – A sequence of Edge objects specifying the edges to seed. The smallest elements will be positioned near edge ends.

• ratio (float) – A Float specifying the ratio of the largest element to the smallest element. Possible values are 1.0 ≤ ratio ≤ 106.

• number (int) – An Int specifying the number of elements along each edge. Possible values are 1 ≤ number ≤ 104.

• minSize (float) – A Float specifying the desired smallest element size.

• maxSize (float) – 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 (SymbolicConstant, default: FREE) –

  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, number, constraint=abaqusConstants.FREE)

This method seeds the given edges uniformly based on the number of elements along the edges.

Note

Check MeshPart.seedEdgeByNumber on help.3ds.com/0.1..

Parameters:

• edges (Tuple[Edge, ...]) – A sequence of Edge objects specifying the edges to seed.

• number (int) – An Int specifying the number of elements along each edge. Possible values are 1 ≤ number ≤ 104.

• constraint (SymbolicConstant, default: FREE) –

  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, size, deviationFactor=None, minSizeFactor=None, constraint=abaqusConstants.FREE)

This method seeds the given edges either uniformly or following edge curvature distribution, based on the desired element size.

Note

Check MeshPart.seedEdgeBySize on help.3ds.com/0.1..

Parameters:

• edges (Tuple[Edge, ...]) – A sequence of Edge objects specifying the edges to seed.

• size (float) – A Float specifying the desired element size.

• deviationFactor (Optional[float], default: None) – A Float specifying the deviation factor h/Lh/L, where hh is the chordal deviation and LL is the element length.

• minSizeFactor (Optional[float], default: None) – A Float specifying the size of the smallest allowable element as a fraction of the specified global element size.

• constraint (SymbolicConstant, default: FREE) –

  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, deviationFactor=None, minSizeFactor=None, constraint=abaqusConstants.FREE)

This method assigns global edge seeds to the given parts.

Note

Check MeshPart.seedPart on help.3ds.com/0.1..

Parameters:

• size (float) – A Float specifying the desired global element size for the edges.

• deviationFactor (Optional[float], default: None) – A Float specifying the deviation factor h/Lh/L, where hh is the chordal deviation and LL is the element length.

• minSizeFactor (Optional[float], default: None) – A Float specifying the size of the smallest allowable element as a fraction of the specified global element size.

• constraint (SymbolicConstant, default: FREE) – 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.

setBoundaryLayerControls(regions, firstElemSize, growthFactor, numLayers, inactiveFaces=(), setName='')

This method sets the control parameters for boundary layer mesh for the specified regions.

Note

Check MeshPart.setBoundaryLayerControls on help.3ds.com/0.1..

Parameters:

• regions (Tuple[Cell, ...]) – A sequence of Cell objects specifying the regions for which to set the boundary layer mesh control parameters.

• firstElemSize (float) – A Float specifying the height of the first element layer off boundary. Possible values are 0.0 << firstElemSize ≤ 106.

• growthFactor (float) – A Float specifying the ratio of heights of any two consecutive element layers. Possible values are 1.0 ≤ growthFactor ≤ 10.0.

• numLayers (int) – An Int specifying the number of element layers to be generated. Possible values are 1 ≤ numLayers ≤ 104.

• inactiveFaces (Tuple[Face, ...], default: ()) – 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 (str, default: '') – A String specifying a unique name for a set that will contain boundary layer elements.

setElementType(regions, elemTypes)

This method assigns element types to the specified regions.

Note

Check MeshPart.setElementType on help.3ds.com/0.1..

Parameters:

• regions (tuple) – 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 (Tuple[ElemType, ...]) – 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:

Exception – 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, corners)

This method sets the logical corners for a mappable face region.

Note

Check MeshPart.setLogicalCorners on help.3ds.com/0.1..

Parameters:

• region (str) – A Face region.

• corners (str) – Three, four, or five ConstrainedSketchVertex objects defining the logical corners for a given mappable face region.

setMeshControls(regions, elemShape=None, technique=None, algorithm=None, minTransition=ON, sizeGrowth=None, allowMapped=OFF)

This method sets the mesh control parameters for the specified regions.

Note

Check MeshPart.setMeshControls on help.3ds.com/0.1..

Parameters:

• regions (tuple) – A sequence of Face or Cell regions specifying the regions for which to set the mesh control parameters.

• elemShape (Optional[SymbolicConstant], default: None) –

  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 (Optional[SymbolicConstant], default: None) –

  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 (Optional[SymbolicConstant], default: None) –

  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 (Union[AbaqusBoolean, bool], default: ON) –

  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 (Optional[SymbolicConstant], default: None) – 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 (Union[AbaqusBoolean, bool], default: OFF) –

  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, edge, sense)

This method sets the sweep path for a sweepable region or the revolve path for a revolvable region.

Note

Check MeshPart.setSweepPath on help.3ds.com/0.1..

Parameters:

• region (str) – A sweepable region.

• edge (Edge) – An Edge object specifying the sweep or revolve path.

• sense (SymbolicConstant) – 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.

verifyMeshQuality(criterion, threshold=None, elemShape=None, regions=())

This method tests the mesh quality of a part and returns poor-quality elements.

Note

Check MeshPart.verifyMeshQuality on help.3ds.com/0.1..

Parameters:

• criterion (SymbolicConstant) –

  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 (Optional[float], default: None) – 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 (Optional[SymbolicConstant], default: None) – A SymbolicConstant specifying an element shape for limiting the query. Possible values are LINE, QUAD, TRI, HEX, WEDGE, and TET.

• regions (tuple, default: ()) – 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) .

Return type:

Dict[str, int | float, MeshElement]

MeshStats

class MeshStats

The MeshStats object is a query object for holding mesh statistics and is returned by the getMeshStats command. The object does not have any methods.

Note

This object can be accessed by:

import mesh

Note

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

Public Data Attributes:

numPointElems	An Int specifying the number of point elements.
numLineElems	An Int specifying the number of line elements.
numQuadElems	An Int specifying the number of quadrilateral elements.
numTriElems	An Int specifying the number of triangular elements.
numHexElems	An Int specifying the number of hexahedral elements.
numWedgeElems	An Int specifying the number of wedge elements.
numTetElems	An Int specifying the number of tetrahedral elements.
numPyramidElems	An Int specifying the number of pyramid elements.
numNodes	An Int specifying the number of nodes.
numMeshedRegions	An Int specifying the number of regions that contain a mesh.

---

numHexElems: Optional[int] = None

An Int specifying the number of hexahedral elements.

numLineElems: Optional[int] = None

An Int specifying the number of line elements.

numMeshedRegions: Optional[int] = None

An Int specifying the number of regions that contain a mesh.

numNodes: Optional[int] = None

An Int specifying the number of nodes.

numPointElems: Optional[int] = None

An Int specifying the number of point elements.

numPyramidElems: Optional[int] = None

An Int specifying the number of pyramid elements.

numQuadElems: Optional[int] = None

An Int specifying the number of quadrilateral elements.

numTetElems: Optional[int] = None

An Int specifying the number of tetrahedral elements.

numTriElems: Optional[int] = None

An Int specifying the number of triangular elements.

numWedgeElems: Optional[int] = None

An Int specifying the number of wedge elements.