Part¶
Features in Abaqus/CAE include Parts, Datums, Partitions, and Assembly operations. Part commands create Feature objects on only the Part object. The commands that create Feature objects on only the rootAssembly object are described in Assembly commands. The commands that create Feature objects on both the Part and the rootAssembly objects are described in Feature commands.
Create parts¶
- class PartModel(
- name,
- description=
'', - stefanBoltzmann=
None, - absoluteZero=
None, - waveFormulation=
NOT_SET, - modelType=
STANDARD_EXPLICIT, - universalGas=
None, - copyConstraints=
1, - copyConnectors=
1, - copyInteractions=
1, Bases:
ModelBaseAbaqus creates a Model object named Model-1 when a session is started.
Note
This object can be accessed by:
mdb.models[name]Note
Public Data Attributes:
Inherited from
ModelBaseA String specifying the repository key.
None or a Float specifying the Stefan-Boltzmann constant.
None or a Float specifying the absolute zero constant.
A SymbolicConstant specifying the type of incident wave formulation to be used in acoustic problems.
None or a Float specifying the universal gas constant.
A Boolean specifying whether an input file should be written without parts and assemblies.
A Boolean specifying that the step specified by restartStep should be terminated at the increment specified by restartIncrement.
A Boolean specifying that a shell global model drives a solid submodel.
A Float specifying the time stamp that indicates when the model was last changed.
A String specifying the purpose and contents of the Model object.
A String specifying the name of the job that generated the restart data.
A String specifying the name of the step where the restart analysis will start.
A String specifying the name of the job that generated the results for the global model.
A boolean specifying the status of constraints created in a model, in the model which instances this model.
A boolean specifying the status of connectors created in a model, in the model which instances this model.
A boolean specifying the status of interactions created in a model, in the model which instances this model.
A KeywordBlock object.
A repository of Amplitude objects.
A repository of Profile objects.
A repository of BoundaryCondition objects.
A repository of ConstrainedSketchConstraint objects.
A repository of AnalyticalField objects.
A repository of DiscreteField objects.
A repository of PredefinedField objects.
A repository of Interaction objects.
A repository of InteractionProperty objects.
A repository of ContactControl objects.
A repository of ContactInitialization objects.
A repository of ContactStabilization objects.
A tuple of tuples of Strings specifying the linked child PartInstance name in the current model to the corresponding parent PartInstance name in a different model.
A tuple of tuples of Strings specifying the linked child Part name in the current model to the corresponding parent Part name in a different model.
A repository of Load objects.
A repository of Material objects.
A repository of Calibration objects.
A repository of Section objects.
A repository of RemeshingRule objects.
A repository of ConstrainedSketch objects.
A repository of Part objects.
A repository of Step objects.
A FeatureOptions object.
A repository of AdaptiveMeshConstraint objects.
A repository of AdaptiveMeshControl objects.
A repository of TimePoint objects.
A repository of Filter objects.
A repository of IntegratedOutputSection objects.
A repository of FieldOutputRequest objects.
A repository of HistoryOutputRequest objects.
A repository of OptimizationTask objects.
A repository of TableCollection objects.
A repository of EventSeriesType objects.
A repository of EventSeriesData objects.
An Int specifying the increment, interval, iteration or cycle where the restart analysis will start.
An Assembly object.
Public Methods:
Part(name, dimensionality, type[, twist])This method creates a Part object and places it in the parts repository.
Inherited from
ModelBase__init__(name[, description, ...])This method creates a Model object.
ModelFromInputFile(name, inputFileName)This method creates a Model object by reading the keywords in an input file and creating the corresponding Abaqus/CAE objects.
ModelFromOdbFile(name, odbFileName)This method creates a Model object by reading an output database and creating any corresponding Abaqus/CAE objects.
ModelFromNastranFile(modelName, inputFileName)This method creates a Model object by reading the keywords in a Nastran bulk data file or Nastran input file and creating any corresponding Abaqus/CAE objects.
setValues([description, noPartsInputFile, ...])This method modifies the Model object.
Member Details:
-
Part(name, dimensionality, type, twist=
0)[source]¶ This method creates a Part object and places it in the parts repository.
Note
This function can be accessed by:
mdb.models[name].PartNote
Check Part on help.3ds.com/2024.
- Parameters:¶
- name¶
A String specifying the repository key.
- dimensionality¶
A SymbolicConstant specifying the dimensionality of the part. Possible values are THREE_D, TWO_D_PLANAR, and AXISYMMETRIC.
- type¶
A SymbolicConstant specifying the type of the part. Possible values are DEFORMABLE_BODY, EULERIAN, DISCRETE_RIGID_SURFACE, and ANALYTIC_RIGID_SURFACE.
- twist=
0¶ A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when dimensionality = AXISYMMETRIC and type = DEFORMABLE_BODY). The default value is OFF.
- Returns:¶
A Part object.
- Return type:¶
-
Part(name, dimensionality, type, twist=
- class PartBase(
- name: str,
- dimensionality: SymbolicConstant,
- type: SymbolicConstant,
- twist: AbaqusBoolean | bool =
OFF, - class PartBase(
- name: str,
- objectToCopy: str,
- scale: float =
1, - mirrorPlane: SymbolicConstant =
NONE, - compressFeatureList: AbaqusBoolean | bool =
OFF, - separate: AbaqusBoolean | bool =
OFF, Bases:
PartFeatureThe Part object defines the physical attributes of a structure. Parts are instanced into the assembly and positioned before an analysis.
Note
This object can be accessed by:
import part mdb.models[name].parts[name]Public Data Attributes:
A Boolean specifying the validity of the geometry of the part.
An Int specifying that feature parameters have been modified but that the part has not been regenerated.
A Float specifying when the part was last modified.
A VertexArray object specifying all the vertices in the part.
An IgnoredVertexArray object specifying all the ignored vertices in the part.
An EdgeArray object specifying all the edges in the part.
An IgnoredEdgeArray object specifying all the ignored edges in the part.
A FaceArray object specifying all the faces in the part.
A CellArray object specifying all the cells in the part.
A repository of Feature objects specifying all the features in the part.
A repository of Feature objects specifying all Feature objects in the part.
A repository of Datum objects specifying all the datums in the part.
A MeshElementArray object specifying all the elements in the part.
A repository of MeshFace objects specifying all the element faces in the part.
A MeshFaceArray object specifying all the unique element faces in the part.
A MeshNodeArray object specifying all the nodes in the part.
A MeshNodeArray object specifying all the retained nodes in the substructure part.
A repository of Set objects specifying for more information, see Set.
A repository of Set objects specifying the contents of the allSets repository is the same as the contents of the sets repository.
A repository of Set objects specifying picked regions.
A repository of Surface objects specifying for more information, see Surface.
A repository of Surface objects specifying the contents of the allSurfaces repository is the same as the contents of the surfaces repository.
A repository of Surface objects specifying picked regions.
A repository of Skin objects specifying the skins created on the part.
A repository of Stringer objects specifying the stringers created on the part.
A repository of ReferencePoint objects.
An EngineeringFeature object.
A SectionAssignmentArray object.
A MaterialOrientationArray object.
A repository of CompositeLayup objects.
A repository of MeshEdge objects specifying all the element edges in the part.
A MeshEdgeArray object specifying all the unique element edges in the part.
nameA String specifying the repository key.
idAn Int specifying the ID of the feature.
Public Methods:
__init__()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.).
This method clears the geometry cache.
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.
This method returns the paths to the associated CAD part and root file.
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.
This method checks if the normal of an analytical rigid surface part is aligned with that of its sketch.
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:
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:
This method returns all regions in the part that do not have a section assignment but require one for analysis.
This method provides a list of all composite plys in the current part which have disjoint regions.
This method regenerates a part.
This method prints any regeneration warnings associated with the features.
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.
This method resumes all the suppressed features in the part.
resumeFeatures(featureNames)This method resumes the specified suppressed features in the part.
This method resumes the last set of features to be suppressed in the part.
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.
This method locks the part for upgrade.
Inherited from
PartFeatureThis 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.
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
FeatureAttachmentPoints(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.
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.
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.
This method queries the suppressed state of the feature.
restore()This method restores the parameters of a feature to the value they had when the backup method was invoked on the part or assembly.
resume()This method resumes suppressed features.
setValues([parameter, parameter1, ...])This method modifies the Feature object.
suppress()This method suppresses features.
Member Details:
- Lock()[source]¶
This method locks the part.
Locking the part prevents any further changes to the part that can trigger regeneration of the part.
- LockForUpgrade()[source]¶
This method locks the part for upgrade.
Locking the part prevents any further changes to the part that can trigger regeneration of the part. When the part is unlocked, all the parts are upgraded and regenrated.
-
Part2DGeomFrom2DMesh(name, part, featureAngle, splineCurvatureLimit=
90, twist=0)[source]¶ This method creates a geometric Part object from the outline of an existing two-dimensional orphan mesh Part object and places it in the parts repository. If the Part2DGeomFrom2DMesh method cannot create a valid two-dimensional shell section from the two-dimensional mesh, the method fails and creates an empty geometry part with a failed base shell feature.
Note
This function can be accessed by:
mdb.models[name].Part2DGeomFrom2DMeshNote
- Parameters:¶
- name¶
A String specifying the repository key.
- part¶
A Part object specifying an existing two-dimensional orphan mesh Part object.
- featureAngle¶
A Float specifying the angle (in degrees) between line segments that triggers a break in the geometry.
- splineCurvatureLimit=
90¶ A Float specifying the traversal angle in degrees of the spline that triggers a break in the geometry. The default value is 90.
- twist=
0¶ A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when dimensionality = AXISYMMETRIC and type = DEFORMABLE_BODY). The default value is OFF.
- Returns:¶
part – A Part object
If the specified part is not an orphan mesh part: Specified part must be an orphan mesh.
If the Part2DGeomFrom2DMesh method cannot create a valid two-dimensional shell section from the two-dimensional mesh: Planar shell feature failed
If the specified part is not two-dimensional: Cannot create a geometry from a 3D part.
If the specified part is a rigid body: Cannot create a geometry from a rigid body.
- Return type:¶
Part
- PartFromBooleanCut(name, instanceToBeCut, cuttingInstances)[source]¶
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.
Note
This function can be accessed by:
mdb.models[name].PartFromBooleanCut
- PartFromBooleanMerge(
- name,
- instances,
- keepIntersections=
False, - mergeNodes=
BOUNDARY_ONLY, - nodeMergingTolerance=
None, - removeDuplicateElements=
1, - domain=
GEOMETRY, This method creates a Part in the parts repository after merging two or more part instances. The part instances can be either Abaqus native parts or orphan mesh parts, but they cannot be a combination of both.
Note
This function can be accessed by:
mdb.models[name].PartFromBooleanMergeNote
- Parameters:¶
- name¶
A String specifying the repository key.
- instances¶
A sequence of PartInstance objects specifying the part instances to merge.
- keepIntersections=
False¶ A Boolean specifying whether the boundary intersections of Abaqus native part instances should be retained after the merge operation. The default value is False.
- mergeNodes=
BOUNDARY_ONLY¶ A SymbolicConstant specifying whether the nodes of orphan mesh part instances should be retained after the merge operation. Possible values are BOUNDARY_ONLY, ALL, or NONE. The default value is BOUNDARY_ONLY.
- nodeMergingTolerance=
None¶ A Float specifying the maximum distance between nodes of orphan mesh part instances that will be merged and replaced with a single new node. The location of the new node is the average position of the deleted nodes. The default value is 10⁻⁶.
- removeDuplicateElements=
1¶ A Boolean specifying whether elements with the same connectivity after the merge will merged into a single element. The default value is ON.
- domain=
GEOMETRY¶ A SymbolicConstant specifying whether the part instances being merged are geometric instances or mesh instances. Possible values are GEOMETRY, MESH or BOTH. The default value is GEOMETRY.
- Returns:¶
part – A Part object
- Return type:¶
Part
- PartFromExtrude2DMesh(name, part, depth, elementSize)[source]¶
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.
Note
This function can be accessed by:
mdb.models[name].PartFromExtrude2DMeshNote
- PartFromGeometryFile(
- name,
- geometryFile,
- dimensionality,
- type,
- bodyNum=
1, - combine=
False, - booleanSolids=
False, - retainBoundary=
False, - usePartNameFromFile=
0, - stitchTolerance=
1, - twist=
0, - scale=
1, - convertToAnalytical=
0, - convertToPrecise=
0, This method creates a Part object and places it in the parts repository.
Note
This function can be accessed by:
mdb.models[name].PartFromGeometryFileNote
- Parameters:¶
- name¶
A String specifying the repository key.
- geometryFile¶
An AcisFile object specifying a file containing geometry.
- dimensionality¶
A SymbolicConstant specifying the dimensionality of the part. Possible values are THREE_D, TWO_D_PLANAR, and AXISYMMETRIC.
- type¶
A SymbolicConstant specifying the type of the part. Possible values are DEFORMABLE_BODY, EULERIAN, DISCRETE_RIGID_SURFACE, and ANALYTIC_RIGID_SURFACE.
- bodyNum=
1¶ An Int specifying the desired body to be selected from an ACIS object containing a list of N ACIS bodies. Possible values are 1 ≤ bodyNum ≤ N. The default value is 1.
- combine=
False¶ A Boolean specifying weather to create a single part by combining all the bodies in the ACIS object. This argument is ignored if bodyNum is specified. The default value is False.
- booleanSolids=
False¶ A Boolean specifying whether the solids should be boolean while combining all the bodies.The default value is FALSE.
- retainBoundary=
False¶ A Boolean specifying whether the intersecting boundaries should be retained while boolean the solids.The default value is FALSE.
- usePartNameFromFile=
0¶ A Boolean specifying whether the part names specified in a STEP file should be used as the names in the Abaqus model database. If this option is TRUE, the part names in the STEP file will be used; if FALSE, each imported part will be named using the text of the name argument followed by a number. This functionality is available only for import from STEP files; for import from all other types of files this option should be FALSE.
- stitchTolerance=
1¶ A Float indicating the maximum gap to be stitched. The value should be smaller than the minimum feature size and bigger than the maximum gap expected to be stitched in the model. Otherwise this command may remove small (sliver) edges that are smaller than the tolerance. The default value is 1.0
- twist=
0¶ A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when dimensionality = AXISYMMETRIC and type = DEFORMABLE_BODY). The default value is OFF.
- scale=
1¶ A Float specifying the scaling factor to apply to the imported geometric entities. The default value is 1.0.
- convertToAnalytical=
0¶ An Int specifying whether to convert to analytical entities. Possible values are 0 or 1. The default value is 0. If convertToAnalytical = 1, all the numerical entities, such as splines, are converted to analytical entities, such as arcs and lines, during the repair phase of the command.
- convertToPrecise=
0¶ An Int specifying whether to convert to precise geometry. Possible value are 0 or 1. The default value is 0. If convertToPrecise = 1, the application will attempt to re-evaluate the tolerant entities to be more precise.
- Returns:¶
part – A Part object
- Return type:¶
Part- Raises:¶
PartError – If the ACIS file is corrupt
PartError – the file is corrupt, If the dimensionality does not correspond to what is found in the ACIS file
PartError – type does not match the contents of the file, dimensionality does not match the contents of the file, If the type does not correspond to what is found in the ACIS file
- PartFromInstanceMesh(
- name,
- partInstances=
(), - copyPartSets=
False, - copyAssemblySets=
False, This method creates a Part object containing the mesh found in the supplied PartInstance objects and places the new Part object in the parts repository.
Note
This function can be accessed by:
mdb.models[name].PartFromInstanceMeshNote
- Parameters:¶
- name¶
A String specifying the repository key.
- partInstances=
()¶ A sequence of PartInstance objects to be used in the creation of the new mesh part. If the partInstances argument is omitted, the new Part object contains the mesh of all the part instances in the assembly.
- copyPartSets=
False¶ A Boolean specifying whether to copy sets, surfaces, and attributes from the base part or parts of the specified part instances to the new part. The default is False.
- copyAssemblySets=
False¶ A Boolean specifying whether to copy assembly-level sets that reference entities of the specified part instances to the new part. The default is False.
- Returns:¶
part – A Part object
If the analysis type (deformable or rigid) is not consistent among the supplied part instances: The selected part instances do not have a consistent analysis type.
If the assembly does not contain a mesh: The current assembly does not contain a mesh for a mesh part.
If the specified part instances do not contain a mesh: The selected part instances do not have a mesh for a mesh part.
- Return type:¶
Part
-
PartFromMesh(name, copySets=
False)[source]¶ This method creates a Part object containing the mesh found in the part and places the new Part object in the parts repository.
Note
This function can be accessed by:
mdb.models[name].PartFromMeshNote
- PartFromMeshMirror(name, part, point1, point2)[source]¶
This method creates a Part object by mirroring an existing orphan mesh Part object about a specified plane and places it in the parts repository. The result is a union of the original and the mirrored copy. Contrast the PartFromMeshMirror method with the mirrorPlane argument of the Part copy constructor. The mirrorPlane argument creates only the second half of the part but does not unite the two halves.
Note
This function can be accessed by:
mdb.models[name].PartFromMeshMirrorNote
- Parameters:¶
- name¶
A String specifying the repository key.
- part¶
A Part object specifying an existing orphan mesh part.
- point1¶
A sequence of three Floats specifying a point on the mirror plane. This point is the local origin in the local system of the plane.
- point2¶
A sequence of three Floats specifying a point in the direction of the normal to the mirror plane. This point must not be coincident with point1.
- Returns:¶
part – A Part object
If the specified part is not an orphan mesh part: Cannot mirror a geometric part.
If the specified part is a rigid body: Cannot mirror a rigid body.
If point1 and point2 are coincident: Mirror plane director has zero length.
If the specified part is two-dimensional and the plane is not parallel to the Z axis: Mirror plane must be parallel to Z axis for 2D parts
- Return type:¶
Part
-
PartFromNodesAndElements(name, dimensionality, type, nodes, elements, twist=
0)[source]¶ This method creates a Part object from nodes and elements and places it in the parts repository.
Note
This function can be accessed by:
mdb.models[name].PartFromNodesAndElementsNote
- Parameters:¶
- name¶
A String specifying the repository key.
- dimensionality¶
A SymbolicConstant specifying the dimensionality of the part. Possible values are THREE_D, TWO_D_PLANAR, and AXISYMMETRIC.
- type¶
A SymbolicConstant specifying the type of the part. Possible values are DEFORMABLE_BODY, EULERIAN, DISCRETE_RIGID_SURFACE, and ANALYTIC_RIGID_SURFACE.
- nodes¶
A sequence of (nodeLabels, nodeCoords) specifying the nodes of the mesh. nodeLabels is a sequence of Ints specifying the node labels, and nodeCoords is a sequence of sequences of three Floats specifying the nodal coordinates.
- elements¶
A sequence of sequences of(meshType, elementLabels, elementConns) specifying the elements of the mesh. meshType is a String specifying the element type. elementlabels is a sequence of Ints specifying the element labels. elementConns is a sequence of sequences of node labels specifying the element connectivity.
- twist=
0¶ A boolean specifying whether the part is defined with twist. This option has meaning only when dimensionality = AXISYMMETRIC. Possible values are ON and OFF. The default value is OFF.
- Returns:¶
part – A Part object
- Return type:¶
Part
- PartFromOdb(
- name,
- odb,
- fileName=
'', - instance=
'', - elementSet=
'', - shape=
UNDEFORMED, - step=
None, - frame=
None, - twist=
0, This method creates an orphan mesh Part object by reading an output database. The new part is placed in the parts repository.
Note
This function can be accessed by:
mdb.models[name].PartFromOdbNote
- Parameters:¶
- name¶
A String specifying the repository key.
- odb¶
An output database object.
- fileName=
''¶ A String specifying the name of the output database file from which to create the part. The default value is an empty string.
- instance=
''¶ A String specifying the part instance in the output database from which to create the part. If no instance name is specified, Abaqus creates an orphan mesh part from the first part instance in the output database.
- elementSet=
''¶ A String specifying an element set defined on the output database. Only elements from this set will be imported. The default is to import all element sets.
- shape=
UNDEFORMED¶ A SymbolicConstant specifying the configuration state. Possible values are UNDEFORMED and DEFORMED. The default value is UNDEFORMED.
- step=
None¶ An Int specifying the step number for reading deformed coordinates. 0≤step≤N−10≤step≤N-1 where NN is the number of available steps. The default value is the last available step. You should specify the step argument only when shape = DEFORMED.
- frame=
None¶ An Int specifying the frame number for reading deformed coordinates. 0≤frame≤N−10≤frame≤N-1 where NN is the number of available frames. The default value is the last available frame. You should specify the frame argument only when shape = DEFORMED.
- twist=
0¶ A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when dimensionality = AXISYMMETRIC and type = DEFORMABLE_BODY). The default value is OFF.
- Returns:¶
part – A Part object
- Return type:¶
Part- Raises:¶
PartError – If the output database contains elements of more than one dimensionality or type: File contains both axisymmetric and nonaxisymmetric elements.File contains both 2D and 3D elements.File contains both rigid and deformable elements. If more than one part is found on the output database:
Error – File does not contain any valid frames. importing of more than one part is not currently supported, - If the output database does not contain any valid results for the specified step:
Error – Specified frame does not contain nodal displacements. If the specified step and frame do not contain any displacements:
Error – Specified element set is not defined in the ODB. If the specified element set is not found on the output database:
OdiError – Invalid step index: i. Available step indices: 0 - j. If the step number is invalid:
OdiError – Invalid frame index: i. Available frame indices: 0 - j. If the frame number is invalid:
- PartFromSection3DMeshByPlane(name, part, point1, point2, point3)[source]¶
This method creates a Part object by cutting an existing three-dimensional orphan mesh Part object by a plane and places it in the parts repository. This method is valid only for orphan mesh parts composed of 8-node brick elements.
Note
This function can be accessed by:
mdb.models[name].PartFromSection3DMeshByPlane- Parameters:¶
- name¶
A String specifying the repository key.
- part¶
A Part object specifying an existing three-dimensional orphan mesh part.
- point1¶
A Sequence of three Floats specifying a point on the cutting plane. This point is the local origin in the local system of the plane.
- point2¶
A Sequence of three Floats specifying a point in the direction of the normal to the cutting plane. This point must not be coincident with point1.
- point3¶
A sequence of three Floats specifying the direction of the local 1-axis in the local system of the plane. This point must not project onto point1.
- Returns:¶
part – A Part object
- Return type:¶
Part- Raises:¶
Exception – If the specified part is not an orphan mesh part, Cannot reduce dimension of a geometric part.
Exception – If the specified part is not three-dimensional, Cannot reduce dimension of a 2D part.
Exception – If the specified part is a rigid body, Cannot change dimension of a rigid body.
Exception – If point1 and point2 are coincident, Cutting plane director has zero length.
Exception – If point3 projects onto point1, Local axis point projects to origin.
Exception – If no elements are cut by the specified plane, Cannot reduce part dimension.
- PartFromSubstructure(name, substructureFile, odbFile)[source]¶
This method creates a substructure Part object by reading a substructure sim file and places it in the parts repository.
Note
This function can be accessed by:
mdb.models[name].PartFromSubstructureNote
- Parameters:¶
- Returns:¶
part – A Part object
- Return type:¶
Part- Raises:¶
Exception – If the specified part is not a substructure, File specified does not contain a substructure.
Exception – If the specified part already exists, A part with the same name already exists.
Exception – If the substructure cannot be imported, The output database is missing nodes and elements.Nested substructures are not supported.The substructure sim file was generated using a version that is different from the current version.
- Unlock()[source]¶
This method unlocks the part.
Unlocking the part allows it to be regenerated after any modifications to the part.
- addGeomToSketch(sketch)[source]¶
This method converts a part into a sketch by projecting all of the edges of the part onto the X-Y plane of the sketch. You can use addGeomToSketch with a part of any modeling space.
Note
-
allInternalSets : --is-rst--:py:class:`dict`\ \[:py:class:`str`, :py:class:`~abaqus.Region.Set.Set`] =
{}[source]¶ A repository of Set objects specifying picked regions.
-
allInternalSurfaces : --is-rst--:py:class:`dict`\ \[:py:class:`str`, :py:class:`~abaqus.Region.Surface.Surface`] =
{}[source]¶ A repository of Surface objects specifying picked regions.
-
allSets : --is-rst--:py:class:`dict`\ \[:py:class:`str`, :py:class:`~abaqus.Region.Set.Set`] =
{}[source]¶ A repository of Set objects specifying the contents of the allSets repository is the same as the contents of the sets repository.
-
allSurfaces : --is-rst--:py:class:`dict`\ \[:py:class:`str`, :py:class:`~abaqus.Region.Surface.Surface`] =
{}[source]¶ A repository of Surface objects specifying the contents of the allSurfaces repository is the same as the contents of the surfaces repository.
-
assignThickness(faces, thickness=
None, topFaces=(), bottomFaces=())[source]¶ This method assigns thickness data to shell faces. The thickness can be used while assigning shell and membrane sections to faces.
Note
- Parameters:¶
- faces¶
A sequence of Face objects specifying the regions where thickness will be applied.
- thickness=
None¶ A Float specifying the thickness along the given faces . Either thickness, topFaces, or bottomFaces must be specified.
- topFaces=
()¶ A sequence of Face objects whose distance to faces argument is used to calculate the thickness along the faces. The combination of topFaces and bottomFaces determines the thickness and the offset of the elements. If bottomFaces is not specified then the thickness is twice the distance to the topFaces. This argument will be ignored if thickness is specified. Either thickness, topFaces, or bottomFaces must be specified.
- bottomFaces=
()¶ A sequence of Face objects whose distance to faces is used to calculate the thickness along the faces. The combination of topFaces and bottomFaces determines the thickness and the offset of the elements. If topFaces is not specified then the thickness is twice the distance to the bottomFaces. This argument will be ignored if thickness is specified. Either thickness, topFaces, or bottomFaces must be specified.
- backup()[source]¶
This method makes a backup copy of the features in the part.
Use the restore method to retrieve the part’s features from the backup.
-
cells : --is-rst--:py:class:`~abaqus.BasicGeometry.CellArray.CellArray` =
[][source]¶ A CellArray object specifying all the cells in the part.
-
checkGeometry(detailed=
0, reportFacetErrors=0, level=None)[source]¶ 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.).
Note
- Parameters:¶
- detailed=
0¶ A Boolean specifying whether detailed output will be printed to the replay file. The default value is OFF.
- reportFacetErrors=
0¶ A Boolean specifying whether faces are checked for proper facetting. The default value is OFF.
- level=
None¶ An Int specifying which level of checking is performed. Values can range from 20 to 70, with higher values reporting less and less important errors. The default value is 20, which reports all critical errors. When the default value is used, the stored validity status is updated to agree with the result of this check.
- detailed=
- clearGeometryCache()[source]¶
This method clears the geometry cache.
Clearing the geometry cache reduces the amount of memory being used to cache part features.
-
compositeLayups : --is-rst--:py:class:`dict`\ \[:py:class:`str`, :py:class:`~abaqus.Property.CompositeLayup.CompositeLayup`] =
{}[source]¶ A repository of CompositeLayup objects.
- copyMeshPattern(elements, faces, elemFaces, targetFace, nodes, coordinates)[source]¶
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.
Note
- Parameters:¶
- elements¶
A sequence of MeshElement objects or a Set object containing elements and specifying the source region.
- faces¶
A sequence of Face objects that have associated with shell elements or element faces and specifying the source region.
- elemFaces¶
A sequence of MeshFace objects specifying the source region.
- targetFace¶
A MeshFace object specifying the target region.
- nodes¶
A sequence of MeshNode objects or a Set object containing nodes on the boundary of source region which are to be positioned to the boundary of target face.
- coordinates¶
A sequence of three-dimensional coordinate tuples specifying the coordinates for each of the given nodes. When specified, the number of coordinate tuples must match the number of given nodes, and be ordered to correspond to the given nodes in ascending order according to index. These coordinates are positions of the nodes of a mesh that will be the target face corresponding to nodes provided.
-
datums : --is-rst--:py:class:`list`\ \[:py:class:`~abaqus.Datum.Datum.Datum`] =
[][source]¶ A repository of Datum objects specifying all the datums in the part.
- deleteFeatures(featureNames)[source]¶
This method deletes the given features.
Note
-
edges : --is-rst--:py:class:`~abaqus.BasicGeometry.EdgeArray.EdgeArray` =
[][source]¶ An EdgeArray object specifying all the edges in the part.
-
elemEdges : --is-rst--:py:class:`dict`\ \[:py:class:`str`, :py:class:`~abaqus.Mesh.MeshEdge.MeshEdge`] =
{}[source]¶ A repository of MeshEdge objects specifying all the element edges in the part. For a given element and a given edge index on a given face within that element, the corresponding MeshEdge object can be retrieved from the repository by using the key calculated as (i*32 + j*4 + k), where i, j, and k are zero-based element, face, and edge indices, respectively.
-
elemFaces : --is-rst--:py:class:`dict`\ \[:py:class:`str`, :py:class:`~abaqus.Mesh.MeshFace.MeshFace`] =
{}[source]¶ A repository of MeshFace objects specifying all the element faces in the part. For a given element and a given face index within that element, the corresponding MeshFace object can be retrieved from the repository by using the key calculated as (i*8 + j), where i and j are zero-based element and face indices, respectively.
-
elementEdges : --is-rst--:py:class:`~abaqus.Mesh.MeshEdgeArray.MeshEdgeArray` =
[][source]¶ A MeshEdgeArray object specifying all the unique element edges in the part.
-
elementFaces : --is-rst--:py:class:`~abaqus.Mesh.MeshFaceArray.MeshFaceArray` =
[][source]¶ A MeshFaceArray object specifying all the unique element faces in the part.
-
elements : --is-rst--:py:class:`~abaqus.Mesh.MeshElementArray.MeshElementArray` =
[][source]¶ A MeshElementArray object specifying all the elements in the part.
-
engineeringFeatures : --is-rst--:py:class:`~abaqus.EngineeringFeature.EngineeringFeature.EngineeringFeature` =
<abaqus.EngineeringFeature.EngineeringFeature.EngineeringFeature object>[source]¶ An EngineeringFeature object.
-
faces : --is-rst--:py:class:`~abaqus.BasicGeometry.FaceArray.FaceArray` =
[][source]¶ A FaceArray object specifying all the faces in the part.
-
features : --is-rst--:py:class:`dict`\ \[:py:class:`str`, :py:class:`~abaqus.Part.PartFeature.PartFeature`] =
{}[source]¶ A repository of Feature objects specifying all the features in the part.
-
featuresById : --is-rst--:py:class:`dict`\ \[:py:class:`str`, :py:class:`~abaqus.Part.PartFeature.PartFeature`] =
{}[source]¶ A repository of Feature objects specifying all Feature objects in the part. The Feature objects in the featuresById repository are the same as the Feature objects in the features’ repository. However, the key to the objects in the featuresById repository is an integer specifying the ID, whereas the key to the objects in the features repository is a string specifying the name.
-
geometryValidity : --is-rst--:py:data:`~typing.Union`\ \[:py:class:`~abaqus.UtilityAndView.AbaqusBoolean.AbaqusBoolean`, :py:class:`bool`] =
0[source]¶ A Boolean specifying the validity of the geometry of the part. The value is computed, but it can be set to ON to perform feature and mesh operations on an invalid part. There is no guarantee that such operations will work if the part was originally invalid.
-
getAngle(plane1, plane2, line1, line2, commonVertex=
'')[source]¶ This method returns the angle between the specified entities.
Note
- Parameters:¶
- plane1¶
A Face, MeshFace, or a Datum object specifying the first plane. The Datum object must represent a datum plane. The plane1 and line1 arguments are mutually exclusive. One of them must be specified.
- plane2¶
A Face, MeshFace, or a Datum object specifying the second plane. The Datum object must represent a datum plane. The plane2 and line2 arguments are mutually exclusive. One of them must be specified.
- line1¶
An Edge, MeshEdge, or a Datum object specifying the first curve. The Datum object must represent a datum axis. The plane1 and line1 arguments are mutually exclusive. One of them must be specified.
- line2¶
An Edge, MeshEdge, or a Datum object specifying the second curve. The Datum object must represent a datum axis. The plane2 and line2 arguments are mutually exclusive. One of them must be specified.
- commonVertex=
''¶ If the two selected Edge objects have more than one vertex in common, this ConstrainedSketchVertex object specifies the vertex at which to evaluate the angle.
- Returns:¶
angle – A Float specifying the angle between the specified entities. If you provide a plane as an argument, Abaqus/CAE computes the angle using the normal to the plane.
- Return type:¶
-
getArea(faces, relativeAccuracy=
0)[source]¶ This method returns the total surface area of a given face or group of faces.
Note
- getAssociatedCADPaths()[source]¶
This method returns the paths to the associated CAD part and root file. These are only available if the part was imported from one of the supported CAD softwares using the Associative Import capability. The root file can be the assembly file or the part file, depending on what which one was imported.
- getCADParameters()[source]¶
This method returns the names and values of the CAD parameters associated with the part. These are only available if the part was imported from one of the supported CAD softwares using the Associative Import capability, and if the parameter names defined in that CAD software are prefixed with the string ABQ.
-
getCentroid(faces, cells, relativeAccuracy=
0)[source]¶ Location of the centroid of a given face/cell or group of faces/cells.
Note
- Parameters:¶
- faces¶
A sequence of Face objects whose centroid the method will calculate. The arguments faces and cells are mutually exclusive.
- cells¶
A sequence of Face objects whose centroid the method will calculate. The arguments faces and cells are mutually exclusive.
- relativeAccuracy=
0¶ A Float specifying that the centroid computation should stop when the specified relative accuracy has been achieved. The default value is 0.000001 (0.0001%).
- Returns:¶
centroid – A sequence of Floats specifying the X, Y, and Z coordinates of the centroid. Depending on the arguments provided, this method returns the following:
The location of the centroid of a given face or group of faces.
The location of the centroid of a given cell or group of cells.
- Return type:¶
Sequence[float]
- getCoordinates(entity, csys)[source]¶
This method returns the coordinates of specified point.
Note
- Parameters:¶
- entity¶
A ConstrainedSketchVertex, Datum point, MeshNode, or ReferencePoint specifying the entity to query.
- csys¶
A DatumCsys object specifying the desired coordinate system of the returned coordinates. By default, coordinates are given in the global coordinate system.
Added in version 2022: The
csysargument was added.
- Returns:¶
A tuple of 3 Floats representing the coordinates of the specified point.
-
getCurvature(edges, samplePoints=
100)[source]¶ This method returns the maximum curvature of a given edge or group of edges. For an arc, the curvature is constant over the entire edge, and equal to the inverse of the radius. For a straight line, the curvature is constant and equal to 0. For a spline edge, the curvature varies over a range, and this methods computes the maximum.
Note
- getDistance(entity1, entity2)[source]¶
Depending on the arguments provided, this method returns one of the following:
The distance between two points.
The minimum distance between a point and an edge.
The minimum distance between two edges.
Note
- getFeatureCells(name)[source]¶
This method returns a sequence of Cell objects that are created by the given feature.
Note
- getFeatureEdges(name)[source]¶
This method returns a sequence of Edge objects that are created by the given feature.
Note
- getFeatureFaces(name)[source]¶
This method returns a sequence of Face objects that are created by the given feature.
Note
- getFeatureVertices(name)[source]¶
This method returns a sequence of ConstrainedSketchVertex objects that are created by the given feature.
Note
- getMassProperties(
- regions=
'', - relativeAccuracy=
LOW, - useMesh=
False, - specifyDensity=
False, - density=
'', - specifyThickness=
False, - thickness=
'', - miAboutCenterOfMass=
True, - miAboutPoint=
(), This method returns the mass properties of a part or region. Only beams, trusses, shells, solids, point, nonstructural mass, and rotary inertia elements are supported.
Note
- Parameters:¶
- regions=
''¶ A MeshElementArray, CellArray, FaceArray, or EdgeArray specifying the regions whose mass properties are to be queried. The whole part is queried by default.
- relativeAccuracy=
LOW¶ A SymbolicConstant specifying the relative accuracy for geometry computation. Possible values are LOW, MEDIUM and HIGH. The default value is LOW.
- useMesh=
False¶ A Boolean specifying whether the mesh should be used in the computation if the geometry is meshed. The default value is False.
- specifyDensity=
False¶ A Boolean specifying whether a user-specified density should be used in regions with density errors such as undefined material density. The default value is False.
- density=
''¶ A double value specifying the user-specified density value to be used in regions with density errors. The user-specified density should be greater than 0.
- specifyThickness=
False¶ A Boolean specifying whether a user-specified thickness should be used in regions with thickness errors such as undefined thickness. The default value is False.
- thickness=
''¶ A double value specifying the user-specified thickness value to be used in regions with thickness errors. The user-specified thickness should be greater than 0.
- miAboutCenterOfMass=
True¶ A Boolean specifying if the moments of inertia should be evaluated about the center of mass. The default value is True.
- miAboutPoint=
()¶ A tuple of three floats specifying the coordinates of the point about which to evaluate the moment of inertia. By default if the moments of inertia are not being evaluated about the center of mass, they will be evaluated about the origin.
- regions=
- Returns:¶
properties – A Dictionary object with the following items:
area: None or a Float specifying the sum of the area of the specified faces. The area is computed only for one side for shells.
areaCentroid: None or a tuple of three Floats representing the coordinates of the area centroid.
volume: None or a Float specifying the volume of the specified regions.
volumeCentroid: None or a tuple of three Floats representing the coordinates of the volume centroid.
massFromMassPerUnitSurfaceArea: None or a Float specifying the mass due to mass per unit surface area.
mass: None or a Float specifying the mass of the specified regions. It is the total mass and includes mass from quantities such as mass per unit surface area.
centerOfMass: None or a tuple of three Floats representing the coordinates of the center of mass.
momentOfInertia: None or a tuple of six Floats representing the moments of inertia about the center of mass or about the point specified.
warnings: A tuple of SymbolicConstants representing the problems encountered while computing the mass properties. Possible SymbolicConstants are:
UNSUPPORTED_ENTITIES: Some unsupported entities exist in the specified region. The mass properties are computed only for beams, trusses, shells, solids, point and non-structural mass elements and rotary inertia elements. The mass properties are not computed for axisymmetric elements, springs, connectors, gaskets or any other elements.
MISSING_THICKNESS: For some regions, the section definitions are missing thickness values.
ZERO_THICKNESS: For some regions, the section definitions have a zero thickness value.
VARIABLE_THICKNESS: The nodal thickness or field thickness specified for some regions has been ignored.
NON_APPLICABLE_THICKNESS: For some regions, the thickness value is not applicable to the corresponding sections specified on the regions.
MISSING_DENSITY: For some regions, the section definitions are missing material density values.
MISSING_MATERIAL_DEFINITION: For some regions, the material definition is missing.
ZERO_DENSITY: For some regions, the section definitions have a zero material density value.
UNSUPPORTED_DENSITY: For some regions, either a negative material density or a temperature dependent density has been specified, or the material value is missing for one or more plies in the composite section.
SHELL_OFFSETS: For shells, this method does not account for any offsets specified.
MISSING_SECTION_DEFINITION: For some regions, the section definition is missing.
UNSUPPORTED_SECTION_DEFINITION: The section definition provided for some regions is not supported.
REINFORCEMENTS: This method does not account for any reinforcements specified on the model.
SMEARED_PROPERTIES: For regions with composite section assignments, the density is smeared across the thickness. The volume centroid and center of mass computations for a composite shell use a lumped mass approach where the volume and mass is assumed to be lumped in the plane of the shell. As a result of these approximations the volume centroid, center of mass and moments of inertia may be slightly inaccurate for regions with composite section assignments.
UNSUPPORTED_NON_STRUCTURAL_MASS_ENTITIES: This method does not account for any non-structural mass on wires.
INCORRECT_MOMENT_OF_INERTIA: For geometry regions with non-structural mass per volume, the non-structural mass is assumed to be a point mass at the centroid of the regions. Thus, the moments of inertia may be inaccurate as the distribution of the non-structural mass is not accounted for. Use the mesh for accurately computing the moments of inertia.
MISSING_BEAM_ORIENTATIONS: For some regions with beam section assignments, the beam section orientations are missing.
UNSUPPORTED_BEAM_PROFILES: This method supports the Box, Pipe, Circular, Rectangular, Hexagonal, Trapezoidal, I, L, T, Arbitrary, and Tapered beam profiles. Any other beam profile is not supported.
TAPERED_BEAM_MI: Moment of inertia calculations for tapered beams are not accurate.
SUBSTRUCTURE_INCORRECT_PROPERTIES: The user assigned density and thickness is not considered for substructures.
UNSUPPORTED_NON_STRUCTURAL_MASS_PROPORTIONAL: Non-structural mass with Mass Proportional distribution is not supported. Results are computed using Volume Proportional distribution.
- Return type:¶
- getPerimeter(faces)[source]¶
This method returns the total perimeter of a given face or group of faces. All faces need to be on the same part. If the specified faces have shared edges, these edges are excluded from the computation, thus providing the length of the outer perimeter of the specified faces.
Note
-
getVolume(cells, relativeAccuracy=
0)[source]¶ This method returns the volume area of a given cell or group of cells.
Note
-
ignoredEdges : --is-rst--:py:class:`~abaqus.BasicGeometry.IgnoredEdgeArray.IgnoredEdgeArray` =
[][source]¶ An IgnoredEdgeArray object specifying all the ignored edges in the part.
-
ignoredVertices : --is-rst--:py:class:`~abaqus.BasicGeometry.IgnoredVertexArray.IgnoredVertexArray` =
[][source]¶ An IgnoredVertexArray object specifying all the ignored vertices in the part.
- isAlignedWithSketch()[source]¶
This method checks if the normal of an analytical rigid surface part is aligned with that of its sketch.
- Returns:¶
A Boolean value of True if the part is aligned with the sketch and False if it is not aligned.
- Return type:¶
Boolean- Raises:¶
AbaqusException – Can only be used with analytical rigid parts, If the part is not an analytical rigid part.
-
isOutOfDate : --is-rst--:py:class:`int` | :py:obj:`None` =
None[source]¶ An Int specifying that feature parameters have been modified but that the part has not been regenerated. Possible values are 0 and 1.
-
materialOrientations : --is-rst--:py:class:`~typing.List`\ \[:py:class:`~abaqus.Property.MaterialOrientation.MaterialOrientation`] =
[][source]¶ A MaterialOrientationArray object.
-
nodes : --is-rst--:py:class:`~abaqus.Mesh.MeshNodeArray.MeshNodeArray` =
[][source]¶ A MeshNodeArray object specifying all the nodes in the part.
- printAssignedSections()[source]¶
This method prints information on each section that has been assigned to a region of the part.
-
projectEdgesOntoSketch(sketch, edges, constrainToBackground=
True)[source]¶ This method projects the selected edges of a part onto the specified ConstrainedSketch object. The edges appear as sketch geometry after projection. If the plane of projection is not parallel to the specified edge, the resultant sketch geometry may be of a different type. For example, a circular edge can be projected as an ellipse or a line depending on the angle of the plane of projection. By default, the projected edge will be constrained to the background geometry. You can remove this constraint by setting constrainToBackground to False.
- Parameters:¶
- projectReferencesOntoSketch(
- sketch,
- filter=
ALL_EDGES, - upToFeature=
None, - edges=
(), - vertices=
(), This method projects the vertices of specified edges, and datum points from the part onto the specified ConstrainedSketch object. The vertices and datum points appear on the sketch as reference geometry.
- Parameters:¶
- sketch¶
The ConstrainedSketch object on which the edges, vertices, and datum points are projected.
- filter=
ALL_EDGES¶ A SymbolicConstant specifying how to limit the amount of projection. Possible values are ALL_EDGES and COPLANAR_EDGES. If filter = COPLANAR_EDGES, edges that are coplanar to the sketching plane are the only candidates for projection. The default value is ALL_EDGES.
- upToFeature=
None¶ A Feature object specifying a marker in the feature-based history of the part. Abaqus/CAE projects onto the sketch only the part entities that were created before the feature specified by this marker. By default, part entities in features created before the sketch you are editing are candidates for projection.
- edges=
()¶ A sequence of candidate edges whose vertices need to be projected onto the sketch. By default, all edges specified by the filter argument are candidates for projection.
- vertices=
()¶ A sequence of candidate vertices to be projected onto the sketch. By default, all vertices are candidates for projection.
-
queryAttributes(printResults=
0)[source]¶ This method prints the following information about a part:
the name, modeling space, and analysis type; and
whether twist is included (only available when the modeling space is axisymmetric and the analysis type is deformable); and
the number of vertices, edges, faces and cells if applicable.
Note
- Parameters:¶
- printResults=
0¶ A Boolean which specifies whether the above information is to be printed. The default value is True
- printResults=
- Returns:¶
attributes – A Dictionary object with string keys and integer values which returns the above information with the keys being numVertices, numEdges, numFaces, numCells, numWiredEdges, numShellFaces and numSolidFaces.
- Return type:¶
- queryCachedStates()[source]¶
This method displays the position of geometric states relative to the sequence of features in the part cache.
The output is displayed in the message area.
- queryDisjointPlyRegions()[source]¶
This method provides a list of all composite plys in the current part which have disjoint regions.
-
queryGeometry(relativeAccuracy=
0, printResults=True)[source]¶ This method prints the following information about a part:
the name, modeling space, and analysis type;
whether twist is included (only available when the modeling space is axisymmetric and the analysis type is deformable);
a 3D point representing the minimum of the part’s bounding box;
a 3D point representing the maximum of the part’s bounding box;
a 3D point representing the part’s centroid (only on 3D solid parts); and
the volume (only on 3D solid parts).
Note
- queryRegionsMissingSections()[source]¶
This method returns all regions in the part that do not have a section assignment but require one for analysis.
-
referencePoints : --is-rst--:py:class:`~abaqus.BasicGeometry.ReferencePoints.ReferencePoints` =
{}[source]¶ A repository of ReferencePoint objects.
- regenerate()[source]¶
This method regenerates a part.
When you modify features, it may be convenient to postpone regeneration until you make all your changes, since regeneration can be time consuming.
- regenerationWarnings()[source]¶
This method prints any regeneration warnings associated with the features.
- removeInvalidGeometry()[source]¶
Removes all invalid entities from the part, leaving a valid part.
This is not recorded as a feature in the feature list, therefore it should be used on parts that have a single feature (such as an imported part). Note:This may remove valid entities that are connected to invalid ones. You can identify invalid entities using the query toolset before using this command.
- restore()[source]¶
This method restores the parameters of all features in the assembly to the value they had before a failed regeneration.
Use the restore method after a failed regeneration, followed by a regenerate command.
- resumeFeatures(featureNames)[source]¶
This method resumes the specified suppressed features in the part.
Note
- resumeLastSetFeatures()[source]¶
This method resumes the last set of features to be suppressed in the part.
-
retainedNodes : --is-rst--:py:class:`~abaqus.Mesh.MeshNodeArray.MeshNodeArray` =
[][source]¶ A MeshNodeArray object specifying all the retained nodes in the substructure part.
- saveGeometryCache()[source]¶
This method caches the current geometry.
Caching the current geometry improves regeneration performance.
-
sectionAssignments : --is-rst--:py:class:`~typing.List`\ \[:py:class:`~abaqus.Property.SectionAssignment.SectionAssignment`] =
[][source]¶ A SectionAssignmentArray object.
-
setAssociatedCADPaths(partFile=
'', rootFile='')[source]¶ This method sets the paths to the associated CAD part and root file. This method is only available if the part was imported from one of the supported CAD softwares using the Associative Import capability. The root file can be the assembly file or the part file, depending on the one that was imported. This method can be used to specify the new paths when the CAD data is moved to a different directory.
-
sets : --is-rst--:py:class:`dict`\ \[:py:class:`str`, :py:class:`~abaqus.Region.Set.Set`] =
{}[source]¶ A repository of Set objects specifying for more information, see Set.
-
skins : --is-rst--:py:class:`dict`\ \[:py:class:`str`, :py:class:`~abaqus.Region.Skin.Skin`] =
{}[source]¶ A repository of Skin objects specifying the skins created on the part.
- smoothNodes(nodes)[source]¶
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.
Note
-
stringers : --is-rst--:py:class:`dict`\ \[:py:class:`str`, :py:class:`~abaqus.Region.Stringer.Stringer`] =
{}[source]¶ A repository of Stringer objects specifying the stringers created on the part.
- suppressFeatures(featureNames)[source]¶
This method suppresses the given features.
Note
-
surfaces : --is-rst--:py:class:`dict`\ \[:py:class:`str`, :py:class:`~abaqus.Region.Surface.Surface`] =
{}[source]¶ A repository of Surface objects specifying for more information, see Surface.
-
timeStamp : --is-rst--:py:class:`float` | :py:obj:`None` =
None[source]¶ A Float specifying when the part was last modified.
-
vertices : --is-rst--:py:class:`~abaqus.BasicGeometry.VertexArray.VertexArray` =
[][source]¶ A VertexArray object specifying all the vertices in the part.
-
writeAcisFile(fileName, version=
None)[source]¶ This method exports the geometry of the part to a named file in ACIS format.
Note
- Parameters:¶
- fileName¶
A String specifying the name of the file to which to write. The file name’s extension is used to determine whether a part or assembly is written. Use the file extension .asat for the assembly format.
Changed in version 2018: Add description for thr file name’s extension.
- version=
None¶ A Float specifying the ACIS version. For example, the Float 12.0 corresponds to ACIS Version 12.0. The default value is the current version of ACIS.
- Raises:¶
Exception – Cannot export orphan mesh parts to ACIS, If the part is an orphan mesh part.
-
writeCADParameters(paramFile, modifiedParams=
(), updatePaths='')[source]¶ This method writes the parameters that were imported from the CAD system to a parameter file.
Note
- Parameters:¶
- paramFile¶
A String specifying the parameter file name.
- modifiedParams=
()¶ A tuple of tuples each containing the part name, the parameter name, and the modified parameter value. Default is an empty tuple.
- updatePaths=
''¶ A Bool specifying whether to update the path of the CAD model file specified in the parameterFile to the current directory, if the CAD model is present in the current directory.
- writeIgesFile(fileName, flavor)[source]¶
This method exports the geometry of the part to a named file in IGES format.
Note
- writeStepFile(fileName)[source]¶
This method exports the geometry of the part to a named file in STEP format.
Note
Other Classes¶
- class AcisFile[source]¶
Bases:
objectThe AcisFile object is a file object used to open ACIS-, STEP-, and IGES-format files.
Note
This object can be accessed by:
import partNote
Member Details:
-
numberOfParts : --is-rst--:py:class:`int` | :py:obj:`None` =
None[source]¶ An Int specifying the number of parts in the object.
-
openAcis(fileName, scaleFromFile=
0)[source]¶ This method creates an AcisFile object from a file containing ACIS-format geometry. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
mdb.openAcisNote
-
openCatia(fileName, topology=
None, convertUnits=0, combineBodies=0)[source]¶ This method creates an AcisFile object from a file containing V5-format geometry. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
mdb.openAcisNote
- Parameters:¶
- fileName¶
A String specifying the path to the CATIA file to open.
- topology=
None¶ A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If topology = SOLID, Abaqus/CAE attempts to attach cells to create a solid. If topology = SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID .
- convertUnits=
0¶ A SymbolicConstant specifying whether the original units should be retained. Possible values are ON and OFF. The default value is OFF.
- combineBodies=
0¶ A Boolean specifying whether to combine the bodies in the CATPart file. If the bodies to be combined touch or overlap, invalid entities would result. For CATProduct files, this option will be ignored.
- Returns:¶
An AcisFile object.
- Return type:¶
-
openEnf(fileName, fileType, topology=
SOLID, convertUnits=0)[source]¶ This method creates an AcisFile object from a file containing Elysium Neutral File-format geometry that was created by CATIA V5, I-DEAS, or Pro/ENGINEER. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
mdb.openAcisNote
- Parameters:¶
- fileName¶
A String specifying the path to the Elysium Neutral File that was created by I-DEAS, Pro/ENGINEER, or CATIA V5.
- fileType¶
A String specifying the type of CAD system that created the file. Possible values are “ideas”, “proe”, or “catiav5” or a combination similar to “proe/ideas/catiav5” if the type is unknown.
- topology=
SOLID¶ A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If topology = SOLID, Abaqus/CAE attempts to attach cells to create a solid. If topology = SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID.
- convertUnits=
0¶ A Boolean specifying if the dimensions of the part should be converted to millimeters. The default value is OFF.
- Returns:¶
An AcisFile object.
- Return type:¶
- openIges(
- fileName,
- trimCurve=
DEFAULT, - scaleFromFile=
0, - msbo=
False, - includedLayers=
(), - topology=
SOLID, - uniteWires=
1, This method creates an AcisFile object from a file containing IGES-format geometry. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
mdb.openAcisNote
- Parameters:¶
- fileName¶
A String specifying the path to the IGES file to open.
- trimCurve=
DEFAULT¶ A SymbolicConstant specifying the method used to define the trim curves that bound parametric surfaces. Possible values are:DEFAULT, use either of the following as specified by the contents of the IGES file.PARAMETRIC_DATA, use the parameter space of the surface being trimmed.THREED_DATA, use real space—the coordinate system of the part along with an indication that the trim curve lies on the parametric surface.The default value is DEFAULT.
- scaleFromFile=
0¶ A SymbolicConstant specifying whether the imported geometry needs to be scaled using the units information available in the IGES file. Possible values are ON and OFF. The default value is OFF. When the argument is set to ON, the geometry is scaled to millimeters with respect to the unit system specified in the IGES file.
- msbo=
False¶ A Boolean specifying if the IGES file contains MSBO (Manifold Solid B-Rep Object) entities. The default value is False.
- includedLayers=
()¶ A sequence of Ints specifying the levels or layers of entities that will be translated from the IGES file to build the part. The default is to include all the layers.
- topology=
SOLID¶ A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If topology = SOLID, Abaqus/CAE attempts to attach cells to create a solid. If topology = SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID.
- uniteWires=
1¶ A SymbolicConstant specifying whether the imported wires need to be united or not. Possible values are ON and OFF. The default value is ON. When importing a sketch, this value is set to OFF.
- Returns:¶
An AcisFile object.
- Return type:¶
- Raises:¶
Texterror – Failed to read IGES file, The data in the IGES file are corrupted.
-
openParasolid(fileName, topology=
SOLID)[source]¶ This method creates an AcisFile object from a file containing Parasolid-format geometry. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
mdb.openAcisNote
- Parameters:¶
- fileName¶
A String specifying the path to the Parasolid file to open.
- topology=
SOLID¶ A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If topology = SOLID, Abaqus/CAE attempts to attach cells to create a solid. If topology = SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID.
- Returns:¶
An AcisFile object.
- Return type:¶
-
openSolidworks(fileName, topology=
SOLID)[source]¶ This method creates an AcisFile object from a file containing Solidworks format geometry. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
mdb.openAcisAdded in version 2020: The
openSolidworksmethod was added.Note
- Parameters:¶
- fileName¶
A String specifying the path to the Solidworks file to open.
- topology=
SOLID¶ A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID, SHELL, and WIRE. If topology = SOLID, Abaqus/CAE attempts to attach cells to create a solid entity. If topology = SHELL, Abaqus/CAE builds the body as a shell entity, not as a solid entity. The default value is SOLID.
- Returns:¶
An AcisFile object.
- Raises:¶
Texterror – Failed to read Solidworks file, The data in the Solidworks file are corrupted.
-
openStep(fileName, scale=
1)[source]¶ This method creates an AcisFile object from a file containing STEP-format geometry. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
mdb.openAcisNote
- openVda(fileName)[source]¶
This method creates an AcisFile object from a file containing VDA-FS-format geometry. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
mdb.openAcisNote
-
writeAcisFile(fileName, version=
None)[source]¶ This method exports the assembly to a named file in ACIS format.
Note
- Parameters:¶
- fileName¶
A String specifying the name of the file to which to write. The file name’s extension is used to determine whether a part or assembly is written. Use the file extension .asat for the assembly format.
Changed in version 2018: Add description for thr file name’s extension.
- version=
None¶ A Float specifying the ACIS version. For example, the Float 12.0 corresponds to ACIS Version 12.0. The default value is the current version of ACIS.
-
numberOfParts : --is-rst--:py:class:`int` | :py:obj:`None` =
-
class AcisMdb(pathName=
'')[source]¶ Bases:
MdbBaseThe Mdb object is the high-level Abaqus model database. A model database stores models and analysis controls.
Note
This object can be accessed by:
mdbNote
Check AcisMdb on help.3ds.com/2024.
Member Details:
-
static openAcis(fileName, scaleFromFile=
0)[source]¶ This method creates an AcisFile object from a file containing ACIS-format geometry. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
mdb.openAcisNote
-
static openCatia(fileName, topology=
None, convertUnits=0, combineBodies=0)[source]¶ This method creates an AcisFile object from a file containing V5-format geometry. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
mdb.openCatiaNote
- Parameters:¶
- fileName¶
A String specifying the path to the CATIA file to open.
- topology=
None¶ A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If topology = SOLID, Abaqus/CAE attempts to attach cells to create a solid. If topology = SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID .
- convertUnits=
0¶ A SymbolicConstant specifying whether the original units should be retained. Possible values are ON and OFF. The default value is OFF.
- combineBodies=
0¶ A Boolean specifying whether to combine the bodies in the CATPart file. If the bodies to be combined touch or overlap, invalid entities would result. For CATProduct files, this option will be ignored.
- Returns:¶
An AcisFile object.
- Return type:¶
AcisFile
-
static openEnf(fileName, fileType, topology=
SOLID, convertUnits=0)[source]¶ This method creates an AcisFile object from a file containing Elysium Neutral File-format geometry that was created by CATIA V5, I-DEAS, or Pro/ENGINEER. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
mdb.openEnfNote
- Parameters:¶
- fileName¶
A String specifying the path to the Elysium Neutral File that was created by I-DEAS, Pro/ENGINEER, or CATIA V5.
- fileType¶
A String specifying the type of CAD system that created the file. Possible values are “ideas”, “proe”, or “catiav5” or a combination similar to “proe/ideas/catiav5” if the type is unknown.
- topology=
SOLID¶ A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If topology = SOLID, Abaqus/CAE attempts to attach cells to create a solid. If topology = SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID.
- convertUnits=
0¶ A Boolean specifying if the dimensions of the part should be converted to millimeters. The default value is OFF.
- Returns:¶
An AcisFile object.
- Return type:¶
AcisFile
- static openIges(
- fileName,
- trimCurve=
DEFAULT, - scaleFromFile=
0, - msbo=
False, - includedLayers=
(), - topology=
SOLID, - uniteWires=
1, This method creates an AcisFile object from a file containing IGES-format geometry. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
mdb.openIgesNote
- Parameters:¶
- fileName¶
A String specifying the path to the IGES file to open.
- trimCurve=
DEFAULT¶ A SymbolicConstant specifying the method used to define the trim curves that bound parametric surfaces. Possible values are:DEFAULT, use either of the following as specified by the contents of the IGES file.PARAMETRIC_DATA, use the parameter space of the surface being trimmed.THREED_DATA, use real space—the coordinate system of the part along with an indication that the trim curve lies on the parametric surface.The default value is DEFAULT.
- scaleFromFile=
0¶ A SymbolicConstant specifying whether the imported geometry needs to be scaled using the units information available in the IGES file. Possible values are ON and OFF. The default value is OFF. When the argument is set to ON, the geometry is scaled to millimeters with respect to the unit system specified in the IGES file.
- msbo=
False¶ A Boolean specifying if the IGES file contains MSBO (Manifold Solid B-Rep Object) entities. The default value is False.
- includedLayers=
()¶ A sequence of Ints specifying the levels or layers of entities that will be translated from the IGES file to build the part. The default is to include all the layers.
- topology=
SOLID¶ A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If topology = SOLID, Abaqus/CAE attempts to attach cells to create a solid. If topology = SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID.
- uniteWires=
1¶ A SymbolicConstant specifying whether the imported wires need to be united or not. Possible values are ON and OFF. The default value is ON. When importing a sketch, this value is set to OFF.
- Returns:¶
An AcisFile object.
- Return type:¶
AcisFile- Raises:¶
Texterror – Failed to read IGES file, The data in the IGES file are corrupted.
-
static openParasolid(fileName, topology=
SOLID)[source]¶ This method creates an AcisFile object from a file containing Parasolid-format geometry. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
mdb.openParasolidNote
- Parameters:¶
- fileName¶
A String specifying the path to the Parasolid file to open.
- topology=
SOLID¶ A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID , SHELL, and WIRE. If topology = SOLID, Abaqus/CAE attempts to attach cells to create a solid. If topology = SHELL, Abaqus/CAE builds the body as a shell entity and not as a solid entity. The default value is SOLID.
- Returns:¶
An AcisFile object.
- Return type:¶
AcisFile
-
static openSolidworks(fileName, topology=
SOLID)[source]¶ This method creates an AcisFile object from a file containing Solidworks format geometry. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
openSolidworksAdded in version 2020: The
openSolidworksmethod was added.Note
- Parameters:¶
- fileName¶
A String specifying the path to the Solidworks file to open.
- topology=
SOLID¶ A SymbolicConstant specifying the topology of the data to be read from the file and of the part to be created. Possible values are SOLID, SHELL, and WIRE. If topology = SOLID, Abaqus/CAE attempts to attach cells to create a solid entity. If topology = SHELL, Abaqus/CAE builds the body as a shell entity, not as a solid entity. The default value is SOLID.
- Returns:¶
An AcisFile object.
- Raises:¶
Texterror – Failed to read Solidworks file, The data in the Solidworks file are corrupted.
-
static openStep(fileName, scale=
1)[source]¶ This method creates an AcisFile object from a file containing STEP-format geometry. This object is subsequently used by the PartFromGeometryFile method.
Note
This function can be accessed by:
mdb.openStepNote
-
static openAcis(fileName, scaleFromFile=
- class Part(
- name: str,
- dimensionality: SymbolicConstant,
- type: SymbolicConstant,
- twist: AbaqusBoolean | bool =
OFF, - class Part(
- name: str,
- objectToCopy: str,
- scale: float =
1, - mirrorPlane: SymbolicConstant =
NONE, - compressFeatureList: AbaqusBoolean | bool =
OFF, - separate: AbaqusBoolean | bool =
OFF, Bases:
BasicGeometryPart,MeshEditPart,MeshPart,PropertyPart,RegionPart,DisplayableThe Part object defines the physical attributes of a structure. Parts are instanced into the assembly and positioned before an analysis.
Note
This object can be accessed by:
import part mdb.models[name].parts[name]Note
Check Part on help.3ds.com/2024.
Member Details:
- class PartFeature[source]¶
Bases:
FeatureThe following commands operate on Feature objects. For more information about the Feature object, see Feature object.
Note
This object can be accessed by:
import partNote
Member Details:
-
AddCells(faceList, flipped=
0)[source]¶ This method tries to convert a shell entity to a solid entity. The conversion is not always successful.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- faceList¶
A sequence of Face objects specifying the faces bounding the cell to add.
- flipped=
0¶ A Boolean specifying the direction of feature creation. The possible values are True and False. The default is True indicating that the direction is opposite to the face normal. When multiple faces are selected, Abaqus attempts to create cells on both sides of the selected faces and ignores the flipped argument.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- AnalyticRigidSurf2DPlanar(sketch)[source]¶
This method creates a first Feature object for an analytical rigid surface by creating a planar wire from the given ConstrainedSketch object.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
-
AnalyticRigidSurfExtrude(sketch, depth=
1)[source]¶ 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.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- AnalyticRigidSurfRevolve(sketch)[source]¶
This method creates a first Feature object for an analytical rigid surface by revolving the given ConstrainedSketch object by 360° about the Y axis.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- AssignMidsurfaceRegion(cellList)[source]¶
This method assign a mid-surface property to sequence of Cell objects. If a reference representation of the part does not exist, it creates one. It also copies the cells to the reference representation and deletes the cells from the active representation of the part.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- AutoRepair()[source]¶
This method carries out a sequence of geometry repair operations if it contains invalid entities. It is expected to improve the geometry, but it does not guarantee that the number of invalid entities will decrease. In some cases, it can also increase the number of invalid entities. Since a number of geometry repair operations and validity checks are performed, it could be a slow operation depending on the complexity of the geometry.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepair
- BaseShell(sketch)[source]¶
This method creates a first Feature object by creating a planar shell from the given ConstrainedSketch object. The ConstrainedSketch object must define a closed profile.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
-
BaseShellExtrude(sketch, depth, draftAngle=
None, pitch=None)[source]¶ This method creates a first Feature object by extruding the given ConstrainedSketch object by the given depth, creating a shell. The ConstrainedSketch object can define either an open or closed profile.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- sketch¶
A ConstrainedSketch object specifying the shape to be extruded.
- depth¶
A Float specifying the extrusion depth. Possible values are Floats > 0.
- draftAngle=
None¶ A Float specifying the draft angle in degrees. Possible values are -90.0 ≤ draftAngle ≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.
- pitch=
None¶ A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are -10⁵ ≤ pitch ≤ 10⁵. The arguments draftAngle and pitch are mutually exclusive.
- Returns:¶
A Feature object.
- Return type:¶
Feature- Raises:¶
RangeError –
- BaseShellRevolve(
- sketch,
- angle,
- pitch=
None, - flipRevolveDirection=
0, - flipPitchDirection=
0, - moveSketchNormalToPath=
0, This method creates a first Feature object by revolving the given ConstrainedSketch object by the given angle, creating a shell. The ConstrainedSketch object can define either an open or closed profile and an axis of revolution. The axis is defined by a single construction line.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- sketch¶
A ConstrainedSketch object specifying the shape to be revolved.
- angle¶
A Float specifying the revolve angle in degrees. Possible values are 0 ≤ angle ≤ 360. Note: If pitch > 0, there is no upper limit for angle.
- pitch=
None¶ A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤ pitch ≤ 10⁵. The default value, 0, implies a normal revolve.
- flipRevolveDirection=
0¶ A Boolean specifying whether to override the direction of feature creation. If flipRevolveDirection = OFF, the default direction of revolution is used. If flipRevolveDirection = ON, the revolve direction is reversed. The default value is OFF.
- flipPitchDirection=
0¶ A Boolean specifying whether to override the direction of translation. If flipPitchDirection = OFF, the direction of translation is given by the direction of the revolve axis. If flipPitchDirection = ON, the translation direction is reversed. The default value is OFF.
- moveSketchNormalToPath=
0¶ A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath = OFF, the sketch plane remains parallel to the revolve axis. If moveSketchNormalToPath = ON, the sketch is moved to match the angle created by the pitch before being revolved. The default value is OFF.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- BaseShellSweep(sketch, path)[source]¶
This method creates a first Feature object by sweeping the given section ConstrainedSketch object along the path defined by the path ConstrainedSketch object, creating a shell. The ConstrainedSketch object can define either an open or closed profile. The origin of the profile sketch is positioned at the start of the sweep path and swept perpendicular to the path. No checks are made for self- intersection.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
-
BaseSolidExtrude(sketch, depth, draftAngle=
None, pitch=None)[source]¶ This method creates a first Feature object by extruding the given ConstrainedSketch object by the given depth, creating a solid. The ConstrainedSketch object must define a closed profile.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- sketch¶
A ConstrainedSketch object specifying the plane shape to be extruded.
- depth¶
A Float specifying the extrusion depth. Possible values are 10^-5 <= depth <= 10^5.
- draftAngle=
None¶ A Float specifying the draft angle in degrees. Possible values are -90.0 ≤ draftAngle ≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.
- pitch=
None¶ A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are -10⁵ ≤ pitch ≤ 10⁵. The arguments draftAngle and pitch are mutually exclusive.
- Returns:¶
A Feature object.
- Return type:¶
Feature
- BaseSolidRevolve(
- sketch,
- angle,
- pitch=
None, - flipRevolveDirection=
0, - flipPitchDirection=
0, - moveSketchNormalToPath=
0, This method creates a first Feature object by revolving the given ConstrainedSketch object by the given angle, creating a solid. The ConstrainedSketch object must define a closed profile and an axis of revolution. The axis is defined by a single construction line.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- sketch¶
A ConstrainedSketch object specifying the shape to be revolved.
- angle¶
A Float specifying the revolve angle in degrees. Possible values are 10⁻⁴ ≤ angle ≤ 360. Note: If pitch > 0, there is no upper limit for angle.
- pitch=
None¶ A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤ pitch ≤ 10⁵. The default value, 0, implies a normal revolve.
- flipRevolveDirection=
0¶ A Boolean specifying whether to override the direction of feature creation. If flipRevolveDirection = OFF, the default direction of revolution is used. If flipRevolveDirection = ON, the revolve direction is reversed. The default value is OFF.
- flipPitchDirection=
0¶ A Boolean specifying whether to override the direction of translation. If flipPitchDirection = OFF, the direction of translation is given by the direction of the revolve axis. If flipPitchDirection = ON, the translation direction is reversed. The default value is OFF.
- moveSketchNormalToPath=
0¶ A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath = OFF, the sketch plane remains parallel to the revolve axis. If moveSketchNormalToPath = ON, the sketch is moved to match the angle created by the pitch before being revolved. The default value is OFF.
- Returns:¶
A Feature object.
- Return type:¶
Feature- Raises:¶
RangeError –
- BaseSolidSweep(sketch, path)[source]¶
This method creates a first Feature object by sweeping the given profile ConstrainedSketch object along the path defined by the path ConstrainedSketch object, creating a solid. The profile ConstrainedSketch object must define a closed profile. The origin of the profile sketch is positioned at the start of the sweep path and swept perpendicular to the path. No checks are made for self- intersection.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- BaseWire(sketch)[source]¶
This method creates a first Feature object by creating a planar wire from the given ConstrainedSketch object.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
-
BlendFaces(side1, side2, method=
None, path=None)[source]¶ This method creates a Feature object by creating new faces that blends two sets of faces.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- side1¶
A sequence of Edge objects specifying one side of the blend. The edges must form a continuous chain without branches.
- side2¶
A sequence of Edge or Face objects specifying the second side of the blend. If side2 contains Edge objects then they must form a continuous chain without branches.
- method=
None¶ A SymbolicConstant indicating a method for creating blends. This argument is a required argument if side2 contains Edge object and it is ignored if side2 contains Faceobjects. It can have one of the following values:TANGENT: The blend is tangent to the sides.SHORTEST_PATH: The blend connects the two sides based on linear interpolation between the two sides.SPECIFY_PATH: The blend connects the two sides along a specified path.
- path=
None¶ An Edge object that connects side1 to side2 and specifies the path for creating the blend. This argument is required if method = SPECIFY_PATH; otherwise, it is ignored.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- Chamfer(length, edgeList)[source]¶
This method creates an additional Feature object by chamfering the given list of edges with a given length.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
Check Chamfer on help.3ds.com/2024.
- ConvertToAnalytical()[source]¶
This method attempts to change entities into a simpler form that will speed up processing and make entities available during feature operations.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepair
-
ConvertToPrecise(method=
RECOMPUTE_GEOMETRY)[source]¶ This method attempts to change imprecise entities so that the geometry becomes precise.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
-
CoverEdges(edgeList, tryAnalytical=
False)[source]¶ This method generates a face using the given edges as the face’s boundaries. The CoverEdges method generates a face by creating the geometry consisting of the underlying surface, associated edges, and vertices.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- Returns:¶
A Feature object.
- Return type:¶
Feature- Raises:¶
Parterror – Cannot find a closed loop, If the given boundary is not a closed loop.
Parterror – Cannot find a closed loop, If the given boundary contains a zero length component.
Parterror – Cannot construct face geometry, If the underlying surface is too difficult to fit.
- Cut( )[source]¶
This method creates an additional Feature object by cutting a hole using the given ConstrainedSketch object.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
Check Cut on help.3ds.com/2024.
- Parameters:¶
- sketchPlane¶
A Datum plane object or a planar Face object.
- sketchPlaneSide¶
A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.
- sketchUpEdge¶
An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.
- sketch¶
A ConstrainedSketch object specifying the planar cut.
- sketchOrientation=
None¶ A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- CutExtrude(
- sketchPlane,
- sketchPlaneSide,
- sketchUpEdge,
- sketchOrientation,
- sketch,
- depth=
None, - upToFace=
'', - draftAngle=
None, - pitch=
None, - flipExtrudeDirection=
0, This method creates an additional Feature object by extruding the given ConstrainedSketch object by the given depth and cutting away material in the solid and shell regions of the part. The ConstrainedSketch object must define a closed profile. The CutExtrude method creates a blind cut (using depth), an up-to-face cut (using upToFace), or a through-all cut (if depth and upToFace are not specified).
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- sketchPlane¶
A Datum plane object or a planar Face object.
- sketchPlaneSide¶
A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.
- sketchUpEdge¶
An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.
- sketchOrientation¶
A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM.
- sketch¶
A ConstrainedSketch object specifying the planar sketch to be extruded.
- depth=
None¶ A Float specifying the extrusion depth. If depth is specified, the cut will be a blind cut. The default is to not specify a depth.
- upToFace=
''¶ A Face specifying the face up to which to cut. If upToFace is specified, the cut will be an up-to-face cut. The default is to not specify a face. Note: If neither depth nor upToFace is specified, the cut will be a through-all cut.
- draftAngle=
None¶ A Float specifying the draft angle in degrees. Possible values are -90.0 ≤ draftAngle ≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.
- pitch=
None¶ A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are -10⁵ ≤ pitch ≤ 10⁵. The arguments draftAngle and pitch are mutually exclusive.
- flipExtrudeDirection=
0¶ A Boolean specifying whether to override the direction of feature creation. If the value is OFF, it means use the direction defined by the sketchPlaneSide; if the value is ON, it means use the opposite direction to the one defined by sketchPlaneSide. The default value is OFF.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- CutLoft(
- loftsections,
- startCondition=
None, - endCondition=
None, - startTangent=
None, - startMagnitude=
None, - endTangent=
None, - endMagnitude=
None, - globalSmoothing=
0, This method creates an additional Feature object by lofting between the given sections and cutting away material from the part. You define the sections using a sequence of edges from the part or an EdgeArray.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
Check CutLoft on help.3ds.com/2024.
- Parameters:¶
- loftsections¶
A sequence of sequences of edges specifying the cross-sections to be lofted. Each outer sequence specifies a section through which the method will pass the loft feature. Each outer sequence can be defined as a sequence of edges or as an EdgeArray. The edges specifying a section must form a simple closed profile and must not contain multiple loops.
- startCondition=
None¶ A SymbolicConstant specifying the tangent direction at the start section of the loft feature. Possible values are NONE, NORMAL, RADIAL, and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the startCondition argument in conjunction with the endCondition argument.
- endCondition=
None¶ A SymbolicConstant specifying the tangent direction at the end section of the loft feature. Possible values are NONE, NORMAL, RADIAL, and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the endCondition argument in conjunction with the startCondition argument.
- startTangent=
None¶ A Float specifying the angle in degrees of the tangent with respect to the plane in which the start section lies. You must specify the startTangent argument if startCondition = SPECIFIED. Possible values are 0.0 ≤ startTangent ≤ 180.0.
- startMagnitude=
None¶ A Float specifying the magnitude of the startTangent. You must specify the startMagnitude argument if startCondition = SPECIFIED. Possible values are 0.0 < startMagnitude < 100.0.
- endTangent=
None¶ A Float specifying the angle in degrees of the tangent with respect to the plane in which the end section lies. You must specify the endTangent argument if startCondition = SPECIFIED. Possible values are 0.0 ≤ endTangent ≤ 180.0.
- endMagnitude=
None¶ A Float specifying the magnitude of the endTangent. This argument is to be used when the endCondition argument has the value SPECIFIED. Possible values are 0.0 < endMagnitude < 100.0.
- globalSmoothing=
0¶ A Boolean specifying whether each path defined in the paths argument is applied locally or globally.If the path is applied locally, its effect is felt only on faces created from the edges on the loftSections through which the paths pass through.If the path is applied globally, an averaging algorithm is applied over all the paths defined and is distributed over all the faces created.The default value is ON (globally).
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- CutRevolve(
- sketchPlane,
- sketchPlaneSide,
- sketchUpEdge,
- sketchOrientation,
- sketch,
- angle,
- pitch=
None, - flipRevolveDirection=
0, - flipPitchDirection=
0, - moveSketchNormalToPath=
0, This method creates an additional Feature object by revolving the given ConstrainedSketch object by the given angle and cutting away material from the part. The ConstrainedSketch object must define a closed profile and an axis of revolution.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- sketchPlane¶
A Datum plane object or a planar Face object.
- sketchPlaneSide¶
A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.
- sketchUpEdge¶
An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.
- sketchOrientation¶
A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM.
- sketch¶
A ConstrainedSketch object specifying the planar sketch to be revolved.
- angle¶
A Float specifying the angle in degrees to be revolved.
- pitch=
None¶ A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤ pitch ≤ 10⁵. The default value, 0, implies a normal revolve.
- flipRevolveDirection=
0¶ A Boolean specifying whether to override the direction of feature creation. If flipRevolveDirection = OFF, the default direction of revolution is used. If flipRevolveDirection = ON, the revolve direction is reversed. The default value is OFF.
- flipPitchDirection=
0¶ A Boolean specifying whether to override the direction of translation. If flipPitchDirection = OFF, the direction of translation is given by the direction of the revolve axis. If flipPitchDirection = ON, the translation direction is reversed. The default value is OFF.
- moveSketchNormalToPath=
0¶ A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath = OFF, the sketch plane remains parallel to the revolve axis. If moveSketchNormalToPath = ON, the sketch is moved to match the angle created by the pitch before being revolved. The default value is OFF.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- CutSweep(
- path,
- profile,
- pathPlane=
'', - pathUpEdge=
None, - pathOrientation=
RIGHT, - sketchPlane=
'', - sketchUpEdge=
None, - sketchOrientation=
RIGHT, - draftAngle=
None, - pitch=
None, - profileNormal=
0, - flipSweepDirection=
0, This method creates an additional Feature object by sweeping the given ConstrainedSketch object along a path which may be a ConstrainedSketch or a sequence of Edge objects and cutting away material from the part. If the profile section is a ConstrainedSketch object, it must define a closed profile. The section sketch can be created at the normal plane at the start of the sweep path or it may be created on a Datum plane or a planar Face. No checks are made for self-intersection.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- path¶
Path may either be a ConstrainedSketch object or a sequence of Edge objects specifying the path of the sweep.
- profile¶
Profile may either be a ConstrainedSketch object or a Face object specifying the section to be swept.
- pathPlane=
''¶ A Datum plane object or a planar Face object. Only required when path is a ConstrainedSketch object.
- pathUpEdge=
None¶ An Edge object or a Datum axis object specifying the vertical (Y) direction of the path sketch. Only required when path is a ConstrainedSketch object.
- pathOrientation=
RIGHT¶ A SymbolicConstant specifying the orientation of pathUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when path is a ConstrainedSketch object.
- sketchPlane=
''¶ A Datum plane object or a planar Face object specifying the plane on which to sketch the profile. Not required when profile is a Face object. When profile is chosen as a ConstrainedSketch object, user may or may not give this as input. If user does not give this as input, the normal plane at the start of the path will be the sketchPlane.
- sketchUpEdge=
None¶ An Edge object or a Datum axis object specifying the vertical (Y) direction of the profile sketch. Only required when profile is a ConstrainedSketch object.
- sketchOrientation=
RIGHT¶ A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when profile is a ConstrainedSketch object.
- draftAngle=
None¶ A Float specifying the draft angle in degrees. Possible values are -90.0 ≤ draftAngle ≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.
- pitch=
None¶ A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are -10⁵ ≤ pitch ≤ 10⁵. The arguments draftAngle and pitch are mutually exclusive.
- profileNormal=
0¶ A Boolean specifying whether to keep the profile normal same as original or varying through out the sweep path. When profileNormal = OFF, the profile normal will vary through out the sweep path. When profileNormal = ON, the profile normal will be same as original through out the sweep path. The default value is OFF.
- flipSweepDirection=
0¶ A Boolean specifying whether to flip the direction in which sweep operation will be performed. When flipSweepDirection = OFF, sweep operation will be performed in the direction of path direction. When flipSweepDirection = ON, sweep operation will be performed in the direction opposite to the path direction. The default value is OFF.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- ExtendFaces(
- faces=
(), - extendAlong=
(), - distance=
None, - upToFaces=
(), - trimToExtendedTargetSurfaces=
True, - upToReferenceRep=
0, This method extends faces along its free edges by offsetting the external edges along the surfaces. One of distance, upToReferenceRep, or upToFaces must be used to specify how far the faces need to be extended.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- faces=
()¶ A sequence of Face objects specifying the faces to be extended. The faces cannot belong to the reference representation. The faces and extendAlong arguments are mutually exclusive. One of them must be specified.
- extendAlong=
()¶ A sequence of Edge objects specifying the edges where to extend the faces. Only free edges are considered. The interior edges will be ignored. The faces and extendAlong arguments are mutually exclusive. One of them must be specified.
- distance=
None¶ A Float indicating the distance to extend the faces along the edges. Either distance, upToReferenceRep, or upToFaces must be specified.
- upToFaces=
()¶ A sequence of Face objects specifying the faces that the selected faces should be extended up to.
- trimToExtendedTargetSurfaces=
True¶ A Boolean indicating that the surfaces of up to target faces should be extended before extending and trimming the selected faces. The default value is True.
- upToReferenceRep=
0¶ A Boolean indicating that the selected faces should be extended along the selected edges and be trimmed along their intersection with the reference representation.
- faces=
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- FaceFromElementFaces(
- elementFaces,
- stitch=
0, - stitchTolerance=
None, - analyticFitTolerance=
None, - associateFace=
0, This method creates a geometry face from a collection of orphan element faces.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- elementFaces¶
A Region object specifying the collection of orphan element faces.
- stitch=
0¶ A Boolean specifying whether the created geometry face should be stitched with existing geometry faces. Default value is TRUE.
- stitchTolerance=
None¶ A Float indicating the maximum gap to be stitched. The value should be smaller than the minimum feature size and bigger than the maximum gap expected to be stitched in the model. Otherwise this command may remove small (sliver) edges that are smaller than the tolerance. If stitch tolerance is not provided then default value of 0.001 will be used for stitching.
- analyticFitTolerance=
None¶ A Float indicating the analytical surface fitting tolerance. If analytical tolerance is not provided then default value of 0.015 will be used for analytical surface fitting.
- associateFace=
0¶ A Boolean specifying whether the created geometry face should be associated with the mesh. Default value is TRUE.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- HoleBlindFromEdges( )[source]¶
This method creates an additional Feature object by creating a circular blind hole of the given diameter and depth and cutting away material in the solid and shell regions of the part. The center of the hole is offset from two non-parallel straight edges by the given distances.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- plane¶
A Datum plane object or a planar Face object.
- planeSide¶
A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.
- diameter¶
A Float specifying the diameter of the hole.
- edge1¶
An Edge object specifying the edge from which distance1 is measured.
- distance1¶
A Float specifying the offset from edge1.
- edge2¶
An Edge object specifying the edge from which distance2 is measured.
- distance2¶
A Float specifying the offset from edge2.
- depth¶
A Float specifying the depth of the hole.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- HoleFromEdges(diameter, edge1, distance1, edge2, distance2)[source]¶
This method creates an additional Feature object by creating a circular hole of the given diameter in a 2D planar part and cutting away material in the shell and wire regions of the part. The center of the hole is offset from two non-parallel straight edges by the given distances.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- diameter¶
A Float specifying the diameter of the hole.
- edge1¶
An Edge object specifying the edge from which distance1 is measured.
- distance1¶
A Float specifying the offset from edge1.
- edge2¶
An Edge object specifying the edge from which distance2 is measured.
- distance2¶
A Float specifying the offset from edge2.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- HoleThruAllFromEdges( )[source]¶
This method creates an additional Feature object by creating a circular through hole of the given diameter and cutting away material in the solid and shell regions of the part. The center of the hole is offset from two non-parallel straight edges by the given distances.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- plane¶
A Datum plane object or a planar Face object.
- planeSide¶
A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.
- diameter¶
A Float specifying the diameter of the hole.
- edge1¶
An Edge object specifying the edge from which distance1 is measured.
- distance1¶
A Float specifying the offset from edge1.
- edge2¶
An Edge object specifying the edge from which distance2 is measured.
- distance2¶
A Float specifying the offset from edge2.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
-
MergeEdges(edgeList=
(), extendSelection=0)[source]¶ This method merges edges either by extending the user selection or using only the selected edges.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
-
Mirror(mirrorPlane, keepOriginal, keepInternalBoundaries=
0)[source]¶ This method mirrors existing part geometry across a plane to create new geometry.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
Check Mirror on help.3ds.com/2024.
- OffsetFaces(
- faceList,
- distance=
None, - targetFaces=
(), - targetFacesMethod=
None, - fractionDistance=
None, - trimToReferenceRep=
0, This method creates new faces by offsetting existing faces.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- faceList¶
A sequence of Face objects specifying the faces that will be offset. The faces may belong to the part or to the reference representation associated with the part.
- distance=
None¶ A Float indicating the distance to offset the faces. Either distance or targetFaces must be specified.
- targetFaces=
()¶ A sequence of Face objects whose distance to the faces argument together with the targetFacesMethod determines the distance to offset the faces. Either distance or targetFaces must be specified.
- targetFacesMethod=
None¶ A SymbolicConstant indicating how to calculate the distance to offset. It can have one of the following values:HALF_OF_AVERAGE: Offset the faces by a distance equals to half the average distance to target faces.CLOSEST_POINT_FRACTION: Offset the faces by a distance equals to the fraction of the distance to the approximate closest point on the selected target faces.FARTHEST_POINT_FRACTION: Offset the faces by a distance equals to the fraction of the distance to the approximate farthest point on the selected target faces.
- fractionDistance=
None¶ A Float indicating the fraction of the distance to the closest or the farthest point on the target faces. Its default value is 0.5.
- trimToReferenceRep=
0¶ A Boolean indicating whether to extend the offset faces and trim them along their intersection with the reference representation.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- RemoveCells(cellList)[source]¶
This method converts a solid entity to a shell entity.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
-
RemoveFaces(faceList, deleteCells=
False)[source]¶ This method removes faces from a solid entity or from a shell entity.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- RemoveFacesAndStitch(faceList)[source]¶
This method removes faces from a solid entity and attempts to close the resulting gap by extending the neighboring faces of the solid.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
-
RemoveRedundantEntities(vertexList=
(), edgeList=(), removeEdgeVertices=True)[source]¶ This method removes redundant edges and vertices from a solid or a shell entity. One of the two arguments is required.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- vertexList=
()¶ A sequence of ConstrainedSketchVertex objects specifying the vertices to be removed.
- edgeList=
()¶ A sequence of Edge objects specifying the edges to be removed.
- removeEdgeVertices=
True¶ A Boolean specifying whether the vertices of the redundant edges need to be removed. The default is True.
- vertexList=
- Returns:¶
A Feature object.
- Return type:¶
Feature- Raises:¶
Parterror – None of the selected entities are redundant, If the selected entity is not a redundant entity.
-
RepairFaceNormals(faceList=
())[source]¶ This method works on the entire part or a sequence of shell faces. When the entire part is selected, it aligns all the shell face normals, and inverts all of the solid faces’ normals if the solid was originally inside out. When a few shell faces are selected, it inverts the normals of the selected faces.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- RepairInvalidEdges(edgeList)[source]¶
This method repairs invalid edges. It will always attempt to improve edges even if none of selected edges are initially invalid and may leave behind invalid edges that could not be repaired.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
-
RepairSliver(face, point1, point2, toleranceChecks=
True)[source]¶ This method repairs the selected sliver from the selected face. The sliver area is specified using two points. A face partition is carried out at the specified points and the smaller of the two faces is removed.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- face¶
A Face object specifying the face on which the sliver is located.
- point1¶
A point specifying the location for partition creation. It can be a ConstrainedSketchVertex object, an Interesting Point or three coordinates specifying the point on an edge of the face.
- point2¶
A point specifying the location for partition creation. It can be a ConstrainedSketchVertex object, an Interesting Point or three coordinates specifying the point on an edge of the face.
- toleranceChecks=
True¶ A Boolean specifying whether to use internal tolerance checks to restrict the size of the sliver face being removed. The default is True.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
-
RepairSmallEdges(edgeList, toleranceChecks=
True)[source]¶ This method repairs small edges. This method will attempt to replace selected small edges with vertices and extend the adjacent faces and edges. This method might leave behind some small edges that cannot be removed.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
-
RepairSmallFaces(faceList, toleranceChecks=
True)[source]¶ This method repairs small faces. It will attempt to replace the selected small faces with edges or vertices and extend the adjacent faces. This method might leave behind some small faces that cannot be removed.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
-
ReplaceFaces(faceList, stitch=
True)[source]¶ This method replaces the selected faces with a single face. If one single face is selected, that alone is replaced with a new face.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Round(radius, edgeList, vertexList)[source]¶
This method creates an additional Feature object by rounding (filleting) the given list of entities with the given radius.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
Check Round on help.3ds.com/2024.
- Parameters:¶
- radius¶
A Float specifying the radius of the fillets.
- edgeList¶
A sequence of Edge objects. Solid and Shell edges of a part can be rounded. The operation will fail for non-manifold edges. The edgeList and vertexList arguments are mutually exclusive. One of them must be specified.
- vertexList¶
A sequence of ConstrainedSketchVertex objects. Vertices that are connected to two wire edges can be rounded. The operation will fail for a vertex connected to a face. The edgeList and vertexList arguments are mutually exclusive. One of them must be specified.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- Shell( )[source]¶
This method creates an additional Feature object by creating a planar shell from the given ConstrainedSketch object. The ConstrainedSketch object must define a closed profile.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
Check Shell on help.3ds.com/2024.
- Parameters:¶
- sketchPlane¶
A Datum plane object or a planar Face object.
- sketchPlaneSide¶
A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.
- sketchUpEdge¶
An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.
- sketch¶
A ConstrainedSketch object specifying the planar shell.
- sketchOrientation=
RIGHT¶ A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- ShellExtrude(
- sketchPlane,
- sketchPlaneSide,
- sketchUpEdge,
- sketch,
- depth=
None, - upToFace=
'', - sketchOrientation=
RIGHT, - draftAngle=
None, - pitch=
None, - flipExtrudeDirection=
0, - keepInternalBoundaries=
0, This method creates an additional Feature object by extruding the given ConstrainedSketch object by the given depth, creating a shell protrusion. The ConstrainedSketch object can define either an open or closed profile.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- sketchPlane¶
A Datum plane object or a planar Face object.
- sketchPlaneSide¶
A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.
- sketchUpEdge¶
An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.
- sketch¶
A ConstrainedSketch object specifying the planar sketch to be extruded.
- depth=
None¶ A Float specifying the extrusion depth. The default is to not specify a depth. Either depth or upToFace must be used to define the extrusion depth.
- upToFace=
''¶ A Face specifying the face up to which to extrude. If upToFace is specified, the extrusion will be an up-to-face extrusion. The default is to not specify a face. Either depth or upToFace must be used to define the extrusion depth.
- sketchOrientation=
RIGHT¶ A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.
- draftAngle=
None¶ A Float specifying the draft angle in degrees. Possible values are -90.0 ≤ draftAngle ≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.
- pitch=
None¶ A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are -10⁵ ≤ pitch ≤ 10⁵. The arguments draftAngle and pitch are mutually exclusive.
- flipExtrudeDirection=
0¶ A Boolean specifying whether to override the direction of feature creation. If the value is OFF, it means use the direction defined by the sketchPlaneSide; if the value is ON, it means use the opposite direction to the one defined by sketchPlaneSide. The default value is OFF.
- keepInternalBoundaries=
0¶ A Boolean specifying whether internal boundaries will be retained. The default value is OFF.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- ShellLoft(
- loftsections,
- startCondition=
None, - endCondition=
None, - startTangent=
None, - startMagnitude=
None, - endTangent=
None, - endMagnitude=
None, - paths=
(), - globalSmoothing=
0, - keepInternalBoundaries=
0, This method creates an additional Feature object by lofting between the given sections and adding shell faces to the part. You define the sections using a sequence of edges from the part or an EdgeArray.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- loftsections¶
A sequence of sequences of edges specifying the cross-sections to be lofted. Each outer sequence specifies a section through which the method will pass the loft feature. Each outer sequence can be defined as a sequence of edges or as an EdgeArray. The edges specifying a section must form a simple closed profile and must not contain multiple loops.
- startCondition=
None¶ A SymbolicConstant specifying the tangent direction at the start section of the loft feature. Possible values are NONE, NORMAL, RADIAL and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the startCondition argument in conjunction with the endCondition argument.
- endCondition=
None¶ A SymbolicConstant specifying the tangent direction at the end section of the loft feature. Possible values are NONE, NORMAL, RADIAL and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the endCondition argument in conjunction with the startCondition argument.
- startTangent=
None¶ A Float specifying the angle in degrees of the tangent with respect to the plane in which the start section lies. You must specify the startTangent argument if startCondition = SPECIFIED. Possible values are 0.0 ≤ startTangent ≤ 180.0.
- startMagnitude=
None¶ A Float specifying the magnitude of the startTangent. You must specify the startMagnitude argument if startCondition = SPECIFIED. Possible values are 0.0 < startMagnitude < 100.0.
- endTangent=
None¶ A Float specifying the angle in degrees of the tangent with respect to the plane in which the end section lies. You must specify the endTangent argument if startCondition = SPECIFIED. Possible values are 0.0 ≤ endTangent ≤ 180.0.
- endMagnitude=
None¶ A Float specifying the magnitude of the endTangent. This argument is to be used when the endCondition argument has the value SPECIFIED. Possible values are 0.0 < endMagnitude < 100.0.
- paths=
()¶ A sequence of sequences of edges that pass through each section in the loft feature. Each sequence specifies a path followed by the face or an edge created by a loft feature. Each path must start at the first section, end at the last section, and pass through each section. In addition, the order of the sequences must be the same as the order of the sections in the loftsections argument. Each path must not self-intersect and must be tangent continuous. In addition, the paths must not intersect each other. You cannot use the paths argument in conjunction with the startCondition and endCondition arguments.
- globalSmoothing=
0¶ A Boolean specifying whether each path defined in the paths argument is applied locally or globally.If the path is applied locally, its effect is felt only on faces created from the edges on the loftsections through which the paths pass through.If the path is applied globally, an averaging algorithm is applied over all the paths defined and is distributed over all the faces created.The default value is ON (globally).
- keepInternalBoundaries=
0¶ A Boolean specifying whether internal boundaries will be retained. The default value is OFF.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- ShellRevolve(
- sketchPlane,
- sketchPlaneSide,
- sketchUpEdge,
- sketch,
- angle,
- sketchOrientation=
RIGHT, - pitch=
None, - flipRevolveDirection=
0, - flipPitchDirection=
0, - moveSketchNormalToPath=
0, - keepInternalBoundaries=
0, This method creates an additional Feature object by revolving the given ConstrainedSketch object by the given angle, creating a shell protrusion. The ConstrainedSketch object can define either an open or closed profile and an axis of revolution. The axis is defined by a single construction line. For a description of the plane positioning arguments, see SolidExtrude.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- sketchPlane¶
A Datum plane object or a planar Face object.
- sketchPlaneSide¶
A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.
- sketchUpEdge¶
An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.
- sketch¶
A ConstrainedSketch object specifying the planar sketch to be revolved.
- angle¶
A Float specifying the angle in degrees to be revolved.
- sketchOrientation=
RIGHT¶ A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.
- pitch=
None¶ A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤ pitch ≤ 10⁵. The default value, 0, implies a normal revolve.
- flipRevolveDirection=
0¶ A Boolean specifying whether to override the direction of feature creation. If flipRevolveDirection = OFF, the default direction of revolution is used. If flipRevolveDirection = ON, the revolve direction is reversed. The default value is OFF.
- flipPitchDirection=
0¶ A Boolean specifying whether to override the direction of translation. If flipPitchDirection = OFF, the direction of translation is given by the direction of the revolve axis. If flipPitchDirection = ON, the translation direction is reversed. The default value is OFF.
- moveSketchNormalToPath=
0¶ A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath = OFF, the sketch plane remains parallel to the revolve axis. If moveSketchNormalToPath = ON, the sketch is moved to match the angle created by the pitch before being revolved. The default value is OFF.
- keepInternalBoundaries=
0¶ A Boolean specifying whether internal boundaries will be retained. The default value is OFF.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- ShellSweep(
- path,
- profile,
- pathPlane=
'', - pathUpEdge=
None, - pathOrientation=
RIGHT, - sketchPlane=
'', - sketchUpEdge=
None, - sketchOrientation=
RIGHT, - draftAngle=
None, - pitch=
None, - profileNormal=
0, - flipSweepDirection=
0, - keepInternalBoundaries=
0, This method creates an additional Feature object by sweeping the given ConstrainedSketch object or a sequence of Edge objects along a path which may be a ConstrainedSketch or a sequence of Edge objects, creating a shell swept protrusion. The section can be an open or a closed profile. The section sketch can be created at the normal plane at the start of the sweep path or it may be created on a Datum plane or a planar Face. No checks are made for self-intersection.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- path¶
Path may either be a ConstrainedSketch object or a sequence of Edge objects specifying the path of the sweep.
- profile¶
Profile may either be a ConstrainedSketch object or a sequence of Edge objects specifying the section to be swept.
- pathPlane=
''¶ A Datum plane object or a planar Face object. Only required when path is a ConstrainedSketch object.
- pathUpEdge=
None¶ An Edge object or a Datum axis object specifying the vertical (Y) direction of the path sketch. Only required when path is a ConstrainedSketch object.
- pathOrientation=
RIGHT¶ A SymbolicConstant specifying the orientation of pathUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when path is a ConstrainedSketch object.
- sketchPlane=
''¶ A Datum plane object or a planar Face object specifying the plane on which to sketch the profile. Not required when profile is a Face object. When profile is chosen as ConstrainedSketch object, user may or may not give this as input. If user does not give this as input, the normal plane at the start of the path will be the sketchPlane.
- sketchUpEdge=
None¶ An Edge object or a Datum axis object specifying the vertical (Y) direction of the profile sketch. Only required when profile is a ConstrainedSketch object.
- sketchOrientation=
RIGHT¶ A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when profile is a ConstrainedSketch object.
- draftAngle=
None¶ A Float specifying the draft angle in degrees. Possible values are -90.0 ≤ draftAngle ≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.
- pitch=
None¶ A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are -10⁵ ≤ pitch ≤ 10⁵. The arguments draftAngle and pitch are mutually exclusive.
- profileNormal=
0¶ A Boolean specifying whether to keep the profile normal same as original or varying through out the sweep path. When profileNormal = OFF, the profile normal will vary through out the sweep path. When profileNormal = ON, the profile normal will be same as original through out the sweep path. The default value is OFF.
- flipSweepDirection=
0¶ A Boolean specifying whether to flip the direction in which sweep operation will be performed. When flipSweepDirection = OFF, sweep operation will be performed in the direction of path direction. When flipSweepDirection = ON, sweep operation will be performed in the direction opposite to the path direction. The default value is OFF.
- keepInternalBoundaries=
0¶ A Boolean specifying whether internal boundaries will be retained. The default value is OFF.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- SolidExtrude(
- sketchPlane,
- sketchPlaneSide,
- sketchUpEdge,
- sketch,
- depth=
None, - upToFace=
None, - sketchOrientation=
RIGHT, - draftAngle=
None, - pitch=
None, - flipExtrudeDirection=
0, - keepInternalBoundaries=
0, This method creates an additional Feature object by extruding the given ConstrainedSketch object by the given depth, creating a solid protrusion. The ConstrainedSketch object must define a closed profile.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- sketchPlane¶
A Datum plane object or a planar Face object.
- sketchPlaneSide¶
A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.
- sketchUpEdge¶
An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.
- sketch¶
A ConstrainedSketch object specifying the planar sketch to be extruded.
- depth=
None¶ A Float specifying the extrusion depth. The default is to not specify a depth. Either depth or upToFace must be used to define the extrusion depth.
- upToFace=
None¶ A Face specifying the face up to which to extrude. If upToFace is specified, the extrusion will be an up-to-face extrusion. The default is to not specify a face. Either depth or upToFace must be used to define the extrusion depth.
- sketchOrientation=
RIGHT¶ A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.
- draftAngle=
None¶ A Float specifying the draft angle in degrees. Possible values are -90.0 ≤ draftAngle ≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.
- pitch=
None¶ A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are -10⁵ ≤ pitch ≤ 10⁵. The arguments draftAngle and pitch are mutually exclusive.
- flipExtrudeDirection=
0¶ A Boolean specifying whether to override the direction of feature creation. If the value is OFF, it means use the direction defined by the sketchPlaneSide; if the value is ON, it means use the opposite direction to the one defined by sketchPlaneSide. The default value is OFF.
- keepInternalBoundaries=
0¶ A Boolean specifying whether internal boundaries will be retained. The default value is OFF.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- SolidLoft(
- loftsections,
- startCondition=
None, - endCondition=
None, - startTangent=
None, - startMagnitude=
None, - endTangent=
None, - endMagnitude=
None, - paths=
(), - globalSmoothing=
0, - keepInternalBoundaries=
0, This method creates an additional Feature object by lofting between the given sections and adding material to the part. You define the sections using a sequence of edges from the part or an EdgeArray.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- loftsections¶
A sequence of sequences of edges specifying the cross-sections to be lofted. Each outer sequence specifies a section through which Abaqus will pass the loft feature. Each outer sequence can be defined as a sequence of edges or as an EdgeArray. The edges specifying a section must form a simple closed profile and must not contain multiple loops.
- startCondition=
None¶ A SymbolicConstant specifying the tangent direction at the start section of the loft feature. Possible values are NONE, NORMAL, RADIAL and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the startCondition argument in conjunction with the endCondition argument.
- endCondition=
None¶ A SymbolicConstant specifying the tangent direction at the end section of the loft feature. Possible values are NONE, NORMAL, RADIAL and SPECIFIED. You can specify this argument only if the start and end sections are planar. You cannot use this argument in conjunction with the path argument. You must use the endCondition argument in conjunction with the startCondition argument.
- startTangent=
None¶ A Float specifying the angle in degrees of the tangent with respect to the plane in which the start section lies. You must specify the startTangent argument if startCondition = SPECIFIED. Possible values are 0.0 ≤ startTangent ≤ 180.0.
- startMagnitude=
None¶ A Float specifying the magnitude of the startTangent. You must specify the startMagnitude argument if startCondition = SPECIFIED. Possible values are 0.0 < startMagnitude < 100.0.
- endTangent=
None¶ A Float specifying the angle in degrees of the tangent with respect to the plane in which the end section lies. You must specify the endTangent argument if startCondition = SPECIFIED. Possible values are 0.0 ≤ endTangent ≤ 180.0.
- endMagnitude=
None¶ A Float specifying the magnitude of the endTangent. This argument is to be used when the endCondition argument has the value SPECIFIED. Possible values are 0.0 < endMagnitude < 100.0.
- paths=
()¶ A sequence of sequences of edges that pass through each section in the loft feature. Each sequence specifies a path followed by the face or an edge created by a loft feature. Each path must start at the first section, end at the last section, and pass through each section. In addition, the order of the sequences must be the same as the order of the sections in the loftsections argument. Each path must not self-intersect and must be tangent continuous. In addition, the paths must not intersect each other. You cannot use the paths argument in conjunction with the startCondition and endCondition arguments.
- globalSmoothing=
0¶ A Boolean specifying whether each path defined in the paths argument is applied locally or globally.If the path is applied locally, its effect is felt only on faces created from the edges on the loftsections through which the paths pass through.If the path is applied globally, an averaging algorithm is applied over all the paths defined and is distributed over all the faces created.The default value is ON (globally).
- keepInternalBoundaries=
0¶ A Boolean specifying whether internal boundaries will be retained. The default value is OFF.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- SolidRevolve(
- sketchPlane,
- sketchPlaneSide,
- sketchUpEdge,
- sketch,
- angle,
- sketchOrientation=
RIGHT, - pitch=
None, - flipRevolveDirection=
0, - flipPitchDirection=
0, - moveSketchNormalToPath=
0, - keepInternalBoundaries=
0, This method creates an additional Feature object by revolving the given ConstrainedSketch object by the given angle, creating a solid protrusion. The ConstrainedSketch object must define a closed profile and an axis of revolution. The axis is defined by a single construction line.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- sketchPlane¶
A Datum plane object or a planar Face object.
- sketchPlaneSide¶
A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.
- sketchUpEdge¶
An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.
- sketch¶
A ConstrainedSketch object specifying the planar sketch to be revolved.
- angle¶
A Float specifying the angle in degrees to be revolved.
- sketchOrientation=
RIGHT¶ A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.
- pitch=
None¶ A Float specifying the pitch. The pitch is the distance traveled along the axial direction, measured between corresponding points on the sketch when it has completed one full revolution about the axis of revolution. Possible values are 0 ≤ pitch ≤ 10⁵. The default value, 0, implies a normal revolve.
- flipRevolveDirection=
0¶ A Boolean specifying whether to override the direction of feature creation. If flipRevolveDirection = OFF, the default direction of revolution is used. If flipRevolveDirection = ON, the revolve direction is reversed. The default value is OFF.
- flipPitchDirection=
0¶ A Boolean specifying whether to override the direction of translation. If flipPitchDirection = OFF, the direction of translation is given by the direction of the revolve axis. If flipPitchDirection = ON, the translation direction is reversed. The default value is OFF.
- moveSketchNormalToPath=
0¶ A Boolean specifying whether to rotate the sketch so that it is normal to the path of revolution when using the pitch option. If moveSketchNormalToPath = OFF, the sketch plane remains parallel to the revolve axis. If moveSketchNormalToPath = ON, the sketch is moved to match the angle created by the pitch before being revolved. The default value is OFF.
- keepInternalBoundaries=
0¶ A Boolean specifying whether internal boundaries will be retained. The default value is OFF.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- SolidSweep(
- path,
- profile,
- pathPlane=
'', - pathUpEdge=
None, - pathOrientation=
RIGHT, - sketchPlane=
'', - sketchUpEdge=
None, - sketchOrientation=
RIGHT, - draftAngle=
None, - pitch=
None, - profileNormal=
0, - flipSweepDirection=
0, - keepInternalBoundaries=
0, This method creates an additional Feature object by sweeping the given ConstrainedSketch object or a Face object along a path which may be a ConstrainedSketch or a sequence of Edge objects, creating a solid swept protrusion. If the profile section is a ConstrainedSketch object, it must define a closed profile. The section sketch can be created at the normal plane at the start of the sweep path or it may be created on a Datum plane or a planar Face. No checks are made for self-intersection.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- path¶
Path may either be a ConstrainedSketch object or a sequence of Edge objects specifying the path of the sweep.
- profile¶
Profile may either be a ConstrainedSketch object or a Face object specifying the section to be swept.
- pathPlane=
''¶ A Datum plane object or a planar Face object. Only required when path is a ConstrainedSketch object.
- pathUpEdge=
None¶ An Edge object or a Datum axis object specifying the vertical (Y) direction of the path sketch. Only required when path is a ConstrainedSketch object.
- pathOrientation=
RIGHT¶ A SymbolicConstant specifying the orientation of pathUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when path is a ConstrainedSketch object.
- sketchPlane=
''¶ A Datum plane object or a planar Face object specifying the plane on which to sketch the profile. Not required when profile is a Face object. When profile is chosen as ConstrainedSketch object, user may or may not give this as input. If user does not give this as input, the normal plane at the start of the path will be the sketchPlane.
- sketchUpEdge=
None¶ An Edge object or a Datum axis object specifying the vertical (Y) direction of the profile sketch. Only required when profile is a ConstrainedSketch object.
- sketchOrientation=
RIGHT¶ A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. Default value is RIGHT. Only required when profile is a ConstrainedSketch object.
- draftAngle=
None¶ A Float specifying the draft angle in degrees. Possible values are -90.0 ≤ draftAngle ≤ 90.0. By convention, for a positive draft angle an outer loop will draft outward and an inner loop will draft inward. The opposite is true for a negative draft angle. The default value, 0, implies a normal extrude. The arguments draftAngle and pitch are mutually exclusive.
- pitch=
None¶ A Float specifying the pitch. The pitch is the distance traveled along the axial direction by the sketch when the sketch has completed one full revolution about the twist axis. Pitch can be specified as positive or negative to achieve right-handed or left-handed twist about the twist axis, respectively. The default value, 0, implies a normal extrude. Possible values are -10⁵ ≤ pitch ≤ 10⁵. The arguments draftAngle and pitch are mutually exclusive.
- profileNormal=
0¶ A Boolean specifying whether to keep the profile normal same as original or varying through out the sweep path. When profileNormal = OFF, the profile normal will vary through out the sweep path. When profileNormal = ON, the profile normal will be same as original through out the sweep path. The default value is OFF.
- flipSweepDirection=
0¶ A Boolean specifying whether to flip the direction in which sweep operation will be performed. When flipSweepDirection = OFF, sweep operation will be performed in the direction of path direction. When flipSweepDirection = ON, sweep operation will be performed in the direction opposite to the path direction. The default value is OFF.
- keepInternalBoundaries=
0¶ A Boolean specifying whether internal boundaries will be retained. The default value is OFF.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
-
Stitch(edgeList=
(), stitchTolerance=None)[source]¶ This method attempts to create a valid part by binding together free and imprecise edges of all the faces of a part. If edgeList is not given, a global stitch will be performed. If stitchTolerance is not specified, a value of 1.0 will be used.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
Check Stitch on help.3ds.com/2024.
- Parameters:¶
- edgeList=
()¶ A sequence of Edge objects specifying the edges that need to be stitched.
- stitchTolerance=
None¶ A Float indicating the maximum gap to be stitched. The value should be smaller than the minimum feature size and bigger than the maximum gap expected to be stitched in the model. Otherwise this command may remove small (sliver) edges that are smaller than the tolerance.
- edgeList=
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- Wire( )[source]¶
This method creates an additional Feature object by creating a planar wire from the given ConstrainedSketch object. The ConstrainedSketch object must define a closed profile.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
Check Wire on help.3ds.com/2024.
- Parameters:¶
- sketchPlane¶
A Datum plane object or a planar Face object specifying the plane on which to sketch.
- sketchPlaneSide¶
A SymbolicConstant specifying the direction of feature creation. Possible values are SIDE1 and SIDE2.
- sketchUpEdge¶
An Edge object or a Datum axis object specifying the vertical (Y) direction of the sketch.
- sketch¶
A ConstrainedSketch object specifying the planar sketch to be revolved.
- sketchOrientation=
RIGHT¶ A SymbolicConstant specifying the orientation of sketchUpEdge on the sketch. Possible values are RIGHT, LEFT, TOP, and BOTTOM. The default value is RIGHT.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
- WireFromEdge(edgeList)[source]¶
This method creates an additional Feature object by creating a Wire by selecting one or more Edge objects of a Solid or Shell part.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
-
WirePolyLine(points, mergeType=
IMPRINT, meshable=1)[source]¶ This method creates an additional Feature object by creating a polyline wire that passes through a sequence of given points. Each point can be a datum point, a vertex, an interesting point, or a tuple.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- points¶
A sequence of ConstrainedSketchVertex, Datum point, or InterestingPoint objects specifying the points through which the polyline wire will pass. points can also be a sequence of tuples of Floats. You must specify at least two values in the sequence.
- mergeType=
IMPRINT¶ A SymbolicConstant specifying the merge behavior of the wire with existing geometry. If mergeType is MERGE, Abaqus merges the wire into solid regions of the part if the wire passes through them. If mergeType is IMPRINT, Abaqus imprints the wire on existing geometry as edges. If mergeType is SEPARATE, Abaqus neither merges nor imprints the spline wire with existing geometry. It creates the wire separately. The default value is IMPRINT.
- meshable=
1¶ A Boolean specifying whether the wire should be available for selection in meshing operations. If meshable = OFF, the wire can be used for connector section assignment. The default value is ON.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
-
WireSpline(points, mergeType=
IMPRINT, smoothClosedSpline=0)[source]¶ This method creates an additional Feature object by creating a spline wire that passes through a sequence of given points. Each point can be a datum point, a vertex, an interesting point, or a tuple.
Note
This function can be accessed by:
mdb.models[name].parts[name].AutoRepairNote
- Parameters:¶
- points¶
A sequence of ConstrainedSketchVertex, Datum point, or InterestingPoint objects specifying the points through which the spline wire will pass. points can also be a sequence of tuples of Floats. You must specify at least two values in the sequence.
- mergeType=
IMPRINT¶ A SymbolicConstant specifying the merge behavior of the wire with existing geometry. If mergeType is MERGE, Abaqus merges the wire into solid regions of the part if the wire passes through them. If mergeType is IMPRINT, Abaqus imprints the spline wire on existing geometry as edges. If mergeType is SEPARATE, Abaqus neither merges nor imprints the spline wire with existing geometry. It creates the wire separately. The default value is IMPRINT.
- smoothClosedSpline=
0¶ A Boolean specifying the behavior of Abaqus when the points defining a spline wire form a closed loop (the start and end points are the same). If smoothClosedSpline = ON, Abaqus creates a smooth spline wire where the tangencies at the end point meet smoothly. If smoothClosedSpline = OFF, Abaqus does not automatically create a smooth end condition. The default value in OFF.
- Returns:¶
feature – A Feature object
- Return type:¶
Feature
-
AddCells(faceList, flipped=