Access
import part mdb.models[name].parts[name]
Part(...)
This method creates a Part object and places it in the parts repository.
Path
mdb.models[name].Part
Required arguments
- 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.
Optional arguments
- twist
A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when dimensionality=AXISYMMETRIC and type=DEFORMABLE_BODY). The default value is OFF.
Return value
A Part object.
Exceptions
InvalidNameError.
Part(...)
This method copies a Part object and places the copy in the parts repository.
Path
mdb.models[name].Part
Required arguments
- name
A String specifying the repository key.
- objectToCopy
A Part Object to be copied.
Optional arguments
- scale
A Float specifying the scaling factor to apply to the imported geometric entities during copy. If a scale is specified, compressFeatureList will be set to ON, regardless of whether it is specified in the command. The default value is 1.
- mirrorPlane
A SymbolicConstant specifying how the part is to be mirrored during copy. Possible values are XYPLANE, XZPLANE, YZPLANE. If a mirror plane is specified, compressFeatureList will be set to ON, regardless of whether it is specified in the command. The default value is NONE.
- compressFeatureList
A Boolean specifying whether to compress the feature list when copying a Part object. The default value is OFF. If mirrorPlane or scale is specified, this argument is ignored.
When you compress the feature, list the resulting part will have a single feature. Any datums or sets in the original part will be lost.
- separate
A Boolean specifying whether to separate disconnected regions into parts. The default value is OFF.
Return value
A Part object.
Exceptions
InvalidNameError.
PartFromBooleanCut(...)
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.
Path
mdb.models[name].rootAssembly.PartFromBooleanCut
Required arguments
- name
A String specifying the repository key.
- instanceToBeCut
A PartInstance specifying the base instance from which to cut other instances.
- cuttingInstances
A sequence of PartInstance objects specifying the instances with which to cut the base instance.
Optional arguments
None.
Return value
A Part object.
Exceptions
InvalidNameError.
PartFromBooleanMerge(...)
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.
Path
mdb.models[name].rootAssembly.PartFromBooleanMerge
Required arguments
- name
A String specifying the repository key.
- instances
A sequence of PartInstance objects specifying the part instances to merge.
Optional arguments
- keepIntersections
A Boolean specifying whether the boundary intersections of Abaqus native part instances should be retained after the merge operation. The default value is False.
- mergeNodes
A SymbolicConstant specifying whether the nodes of orphan mesh part instances should be retained after the merge operation. Possible values are BOUNDARY_ONLY, ALL, or NONE. The default value is BOUNDARY_ONLY.
- nodeMergingTolerance
A Float specifying the maximum distance between nodes of orphan mesh part instances that will be merged and replaced with a single new node. The location of the new node is the average position of the deleted nodes. The default value is 10–6.
- removeDuplicateElements
A Boolean specifying whether elements with the same connectivity after the merge will merged into a single element. The default value is ON.
- domain
A SymbolicConstant specifying whether the part instances being merged are geometric instances or mesh instances. Possible values are GEOMETRY, MESH or BOTH. The default value is GEOMETRY.
Return value
A Part object.
Exceptions
InvalidNameError.
PartFromExtrude2DMesh(...)
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.
Path
mdb.models[modelName].PartFromExtrude2DMesh
Required arguments
- name
A String specifying the repository key.
- part
A Part object specifying an existing two-dimensional orphan mesh Part object.
- depth
A Float specifying the total extrusion distance.
- elementSize
A Float specifying an approximate element length in the extruded direction.
Optional arguments
None.
Return value
A Part object.
Exceptions
InvalidNameError.
- If the specified part is not an orphan mesh part:
Cannot extrude a geometric part.
- If the specified part is not two-dimensional:
Cannot extrude a 3D part.
- If the specified part is a rigid body:
Cannot change dimension of a rigid body.
PartFromGeometryFile(...)
This method creates a Part object and places it in the parts repository.
Path
mdb.models[modelName].PartFromGeometryFile
Required arguments
- 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.
Optional arguments
- bodyNum
An Int specifying the desired body to be selected from an ACIS object containing a list of N ACIS bodies. Possible values are 1 bodyNum N. The default value is 1.
- combine
A Boolean specifying weather to create a single part by combining all the bodies in the ACIS object. This argument is ignored if bodyNum is specified. The default value is False.
- booleanSolids
A Boolean specifying whether the solids should be boolean while combining all the bodies.The default value is FALSE.
- retainBoundary
A Boolean specifying whether the intersecting boundaries should be retained while boolean the solids.The default value is FALSE.
- usePartNameFromFile
A Boolean specifying whether the part names specified in a STEP file should be used as the names in the Abaqus model database. If this option is TRUE, the part names in the STEP file will be used; if FALSE, each imported part will be named using the text of the name argument followed by a number. This functionality is available only for import from STEP files; for import from all other types of files this option should be FALSE.
- stitchTolerance
A Float indicating the maximum gap to be stitched. The value should be smaller than the minimum feature size and bigger than the maximum gap expected to be stitched in the model. Otherwise this command may remove small (sliver) edges that are smaller than the tolerance. The default value is 1.0
- twist
A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when dimensionality=AXISYMMETRIC and type=DEFORMABLE_BODY). The default value is OFF.
- scale
A Float specifying the scaling factor to apply to the imported geometric entities. The default value is 1.0.
- convertToAnalytical
An Int specifying whether to convert to analytical entities. Possible values are 0 or 1. The default value is 0. If convertToAnalytical=1, all the numerical entities, such as splines, are converted to analytical entities, such as arcs and lines, during the repair phase of the command.
- convertToPrecise
An Int specifying whether to convert to precise geometry. Possible value are 0 or 1. The default value is 0. If convertToPrecise=1, the application will attempt to re-evaluate the tolerant entities to be more precise.
Return value
A Part object.
Exceptions
InvalidNameError.
- If the ACIS file is corrupt:
PartError: the file is corrupt
- If the dimensionality does not correspond to what is found in the ACIS file:
PartError: dimensionality does not match the contents of the file
- If the type does not correspond to what is found in the ACIS file:
PartError: type does not match the contents of the file
PartFromInstanceMesh(...)
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.
Path
mdb.models[name].rootAssembly.PartFromInstanceMesh
Required arguments
- name
A String specifying the repository key.
Optional arguments
- partInstances
A sequence of PartInstance objects to be used in the creation of the new mesh part. If the partInstances argument is omitted, the new Part object contains the mesh of all the part instances in the assembly.
- copyPartSets
A Boolean specifying whether to copy sets, surfaces, and attributes from the base part or parts of the specified part instances to the new part. The default is False.
- copyAssemblySets
A Boolean specifying whether to copy assembly-level sets that reference entities of the specified part instances to the new part. The default is False.
Return value
A Part object.
Exceptions
InvalidNameError.
- 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.
PartFromMesh(...)
This method creates a Part object containing the mesh found in the part and places the new Part object in the parts repository.
Path
mdb.models[name].parts[name].PartFromMesh
Required arguments
- name
A String specifying the repository key.
Optional arguments
- copySets
A Boolean specifying whether to copy sets, surfaces, and attributes to the new part. The default is False.
Return value
A Part object.
Exceptions
InvalidNameError.
- If the part does not contain a mesh:
The current part does not contain a mesh for a mesh part.
PartFromMeshMirror(...)
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.
Path
mdb.models[modelName].PartFromMeshMirror
Required arguments
- 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.
Optional arguments
None.
Return value
A Part object.
Exceptions
InvalidNameError.
- 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
PartFromNodesAndElements(...)
This method creates a Part object from nodes and elements and places it in the parts repository.
Path
mdb.models[modelName].PartFromNodesAndElements
Required arguments
- 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.
Optional arguments
- twist
A boolean specifying whether the part is defined with twist. This option has meaning only when dimensionality=AXISYMMETRIC. Possible values are ON and OFF. The default value is OFF.
Return value
A Part object.
Exceptions
None.
PartFromOdb(...)
This method creates an orphan mesh Part object by reading an output database. The new part is placed in the parts repository.
Path
mdb.models[modelName].PartFromOdb
Required arguments
- name
A String specifying the repository key.
- odb
An output database object.
Optional arguments
- fileName
A String specifying the name of the output database file from which to create the part. The default value is an empty string.
- instance
A String specifying the part instance in the output database from which to create the part. If no instance name is specified, Abaqus creates an orphan mesh part from the first part instance in the output database.
- elementSet
A String specifying an element set defined on the output database. Only elements from this set will be imported. The default is to import all element sets.
- shape
A SymbolicConstant specifying the configuration state. Possible values are UNDEFORMED and DEFORMED. The default value is UNDEFORMED.
- step
An Int specifying the step number for reading deformed coordinates. where is the number of available steps. The default value is the last available step. You should specify the step argument only when shape=DEFORMED.
- frame
An Int specifying the frame number for reading deformed coordinates. where is the number of available frames. The default value is the last available frame. You should specify the frame argument only when shape=DEFORMED.
- twist
A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when dimensionality=AXISYMMETRIC and type=DEFORMABLE_BODY). The default value is OFF.
Return value
A Part object.
Exceptions
InvalidNameError.
- If the output database contains elements of more than one dimensionality or type:
File contains both axisymmetric and nonaxisymmetric elements.
File contains both 2D and 3D elements.
File contains both rigid and deformable elements.
- If more than one part is found on the output database:
PartError: importing of more than one part is not currently supported
- If the output database does not contain any valid results for the specified step:
Error. File does not contain any valid frames.
- If the specified step and frame do not contain any displacements:
Error. Specified frame does not contain nodal displacements.
- If the specified element set is not found on the output database:
Error. Specified element set is not defined in the ODB.
- If the step number is invalid:
OdiError: Invalid step index: i. Available step indices: 0 - j.
- If the frame number is invalid:
OdiError: Invalid frame index: i. Available frame indices: 0 - j.
PartFromSection3DMeshByPlane(...)
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.
Path
mdb.models[modelName].PartFromSection3DMeshByPlane
Required arguments
- 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.
Optional arguments
None.
Return value
A Part object.
Exceptions
InvalidNameError.
- If the specified part is not an orphan mesh part:
Cannot reduce dimension of a geometric part.
- If the specified part is not three-dimensional:
Cannot reduce dimension of a 2D part.
- If the specified part is a rigid body:
Cannot change dimension of a rigid body.
- If point1 and point2 are coincident:
Cutting plane director has zero length.
- If point3 projects onto point1:
Local axis point projects to origin.
- If no elements are cut by the specified plane:
Cannot reduce part dimension.
PartFromSubstructure(...)
This method creates a substructure Part object by reading a substructure sim file and places it in the parts repository.
Path
mdb.models[name].PartFromSubstructure
Required arguments
- name
A String specifying the repository key.
- substructureFile
A substructure sim file.
- odbFile
The output database file corresponding to the substructure sim file.
Optional arguments
None.
Return value
A Part object.
Exceptions
InvalidNameError.
- If the specified part is not a substructure:
File specified does not contain a substructure.
- If the specified part already exists:
A part with the same name already exists.
- If the substructure cannot be imported:
The output database is missing nodes and elements.
Nested substructures are not supported.
The substructure sim file was generated using a version that is different from the current version.
Part2DGeomFrom2DMesh(...)
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.
Path
mdb.models[modelName].Part2DGeomFrom2DMesh
Required arguments
- 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.
Optional arguments
- splineCurvatureLimit
A Float specifying the traversal angle in degrees of the spline that triggers a break in the geometry. The default value is 90.
- twist
A Boolean specifying whether to include a twist DEGREE OF FREEDOM in the part (only available when dimensionality=AXISYMMETRIC and type=DEFORMABLE_BODY). The default value is OFF.
Return value
A Part object.
Exceptions
InvalidNameError.
- 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.
setValues(...)
This method modifies the Part object.
Required arguments
None.
Optional arguments
The optional arguments to setValues are the same as the arguments to the Part method. In addition, setValues has the following optional argument:
- geometryRefinement
A SymbolicConstant specifying how the part's surface is being refined when faceted for display. Possible values are EXTRA_COARSE, COARSE, MEDIUM, FINE, and EXTRA_FINE.
- startNodeLabel
A positive Integer specifying the new start node label for the part mesh that currently exists or will be generated. If the part is meshed, Abaqus/CAE changes the node labels while preserving the original order and incrementation.
- startElemLabel
A positive Integer specifying the new start element label for the part mesh that currently exists or will be generated. If the part is meshed, Abaqus/CAE changes the element labels while preserving the original order and incrementation.
Return value
None.
Exceptions
RangeError.
addGeomToSketch(...)
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.
Required arguments
- sketch
A ConstrainedSketch object.
Optional arguments
None.
Return value
None.
Exceptions
None.
assignThickness(...)
This method assigns thickness data to shell faces. The thickness can be used while assigning shell and membrane sections to faces.
Required arguments
- faces
A sequence of Face objects specifying the regions where thickness will be applied.
Optional arguments
- thickness
A Float specifying the thickness along the given faces . Either thickness, topFaces, or bottomFaces must be specified.
- topFaces
A sequence of Face objects whose distance to faces argument is used to calculate the thickness along the faces. The combination of topFaces and bottomFaces determines the thickness and the offset of the elements. If bottomFaces is not specified then the thickness is twice the distance to the topFaces. This argument will be ignored if thickness is specified. Either thickness, topFaces, or bottomFaces must be specified.
- bottomFaces
A sequence of Face objects whose distance to faces is used to calculate the thickness along the faces. The combination of topFaces and bottomFaces determines the thickness and the offset of the elements. If topFaces is not specified then the thickness is twice the distance to the bottomFaces. This argument will be ignored if thickness is specified. Either thickness, topFaces, or bottomFaces must be specified.
Return value
None.
Exceptions
None.
backup()
This method makes a backup copy of the features in the part. Use the restore method to retrieve the part's features from the backup.
Arguments
None.
Return value
None.
Exceptions
None.
checkGeometry(...)
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.).
Required arguments
None.
Optional arguments
- detailed
A Boolean specifying whether detailed output will be printed to the replay file. The default value is OFF.
- reportFacetErrors
A Boolean specifying whether faces are checked for proper facetting. The default value is OFF.
- level
An Int specifying which level of checking is performed. Values can range from 20 to 70, with higher values reporting less and less important errors. The default value is 20, which reports all critical errors. When the default value is used, the stored validity status is updated to agree with the result of this check.
Return value
None.
Exceptions
None.
clearGeometryCache()
This method clears the geometry cache. Clearing the geometry cache reduces the amount of memory being used to cache part features.
Arguments
None.
Return value
None.
Exceptions
None.
deleteAllFeatures()
This method deletes all the features in the part.
Arguments
None.
Return value
None.
Exceptions
None.
deleteFeatures(...)
This method deletes the given features.
Required arguments
- featureNames
A sequence of Strings specifying the feature names that will be deleted from the part.
Optional arguments
None.
Return value
None.
Exceptions
None.
getAngle(...)
This method returns the angle between the specified entities.
Required arguments
- 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.
Optional arguments
Return value
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.
Exceptions
None.
getArea(...)
This method returns the total surface area of a given face or group of faces.
Required arguments
- faces
A sequence of face objects whose area the method will calculate.
Optional arguments
- relativeAccuracy
A Float specifying that the area computation should stop when the specified relative accuracy has been achieved. The default value is 0.000001 (0.0001%).
Return value
A Float specifying the sum of the calculated areas of the given faces.
Exceptions
None.
getAssociatedCADPaths()
This method returns the paths to the associated CAD part and root file. These are only available if the part was imported from one of the supported CAD softwares using the Associative Import capability. The root file can be the assembly file or the part file, depending on what which one was imported.
Arguments
None.
Return value
A sequence containing the path to the associated CAD part and assembly file.
Exceptions
None.
getCADParameters()
This method returns the names and values of the CAD parameters associated with the part. These are only available if the part was imported from one of the supported CAD softwares using the Associative Import capability, and if the parameter names defined in that CAD software are prefixed with the string ABQ.
Arguments
None.
Return value
A dictionary object representing a map of the name of the parameter and its associated value.
Exceptions
None.
getCentroid(...)
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.
Required arguments
- 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.
Optional arguments
- relativeAccuracy
A Float specifying that the centroid computation should stop when the specified relative accuracy has been achieved. The default value is 0.000001 (0.0001%).
Return value
A sequence of Floats specifying the X-, Y-, and Z-coordinates of the centroid.
Exceptions
None.
getCoordinates(...)
This method returns the coordinates of specified point.
Required arguments
- entity
A Vertex, Datum point, MeshNode, or ReferencePoint specifying the entity to query.
Optional arguments
None.
Return value
A tuple of 3 Floats representing the coordinates of the specified point.
Exceptions
None.
getCurvature(...)
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.
Required arguments
- edges
A sequence of edge objects whose curvature the method will calculate.
Optional arguments
- samplePoints
An Int specifying the number of points along each edge at which the curvature will be computed. The higher the number of sample points, the better the accuracy of the computation. The default value is 100.
Return value
A Float specifying the maximum curvature.
Exceptions
None.
getDistance(...)
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.
Required arguments
Optional arguments
None.
Return value
A Float specifying the distance between entity1 and entity2.
Exceptions
None.
getLength(...)
This method returns the length of a given edge or group of edges.
Required arguments
- edges
A sequence of edge objects whose total length the method will calculate.
Optional arguments
None.
Return value
A Float specifying the total length.
Exceptions
None.
getPerimeter(...)
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.
Required arguments
- faces
A sequence of face objects whose perimeter the method will calculate.
Optional arguments
None.
Return value
A Float specifying the perimeter.
Exceptions
None.
getVolume(...)
This method returns the volume area of a given cell or group of cells.
Required arguments
- cells
A sequence of cell objects whose volume the method will calculate.
Optional arguments
- relativeAccuracy
A Float specifying the relative accuracy of the computation. The default value is 0.000001 (0.0001%).
Return value
A Float specifying the sum of the areas of the given faces.
Exceptions
None.
getMassProperties(...)
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.
Required arguments
None.
Optional arguments
- regions
A MeshElementArray, CellArray, FaceArray, or EdgeArray specifying the regions whose mass properties are to be queried. The whole part is queried by default.
- relativeAccuracy
A SymbolicConstant specifying the relative accuracy for geometry computation. Possible values are LOW, MEDIUM and HIGH. The default value is LOW.
- useMesh
A Boolean specifying whether the mesh should be used in the computation if the geometry is meshed. The default value is False.
- specifyDensity
A Boolean specifying whether a user-specified density should be used in regions with density errors such as undefined material density. The default value is False.
- density
A double value specifying the user-specified density value to be used in regions with density errors. The user-specified density should be greater than 0.
- specifyThickness
A Boolean specifying whether a user-specified thickness should be used in regions with thickness errors such as undefined thickness. The default value is False.
- thickness
A double value specifying the user-specified thickness value to be used in regions with thickness errors. The user-specified thickness should be greater than 0.
- miAboutCenterOfMass
A Boolean specifying if the moments of inertia should be evaluated about the center of mass. The default value is True.
- miAboutPoint
A tuple of three floats specifying the coordinates of the point about which to evaluate the moment of inertia. By default if the moments of inertia are not being evaluated about the center of mass, they will be evaluated about the origin.
Return value
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.
Exceptions
None.
getFeatureFaces(...)
This method returns a sequence of Face objects that are created by the given feature.
Required arguments
- name
A string specifying the feature name.
Optional arguments
None.
Return value
Sequence of Face objects.
Exceptions
- An exception occurs if a feature with the given name does not exist.
Error : Incorrect feature name.
getFeatureEdges(...)
This method returns a sequence of Edge objects that are created by the given feature.
Required arguments
- name
A string specifying the feature name.
Optional arguments
None.
Return value
Sequence of Edge objects.
Exceptions
- An exception occurs if a feature with the given name does not exist.
Error : Incorrect feature name.
getFeatureCells(...)
This method returns a sequence of Cell objects that are created by the given feature.
Required arguments
- name
A string specifying the feature name.
Optional arguments
None.
Return value
Sequence of Cell objects.
Exceptions
- An exception occurs if a feature with the given name does not exist.
Error : Incorrect feature name.
getFeatureVertices(...)
This method returns a sequence of Vertex objects that are created by the given feature.
Required arguments
- name
A string specifying the feature name.
Optional arguments
None.
Return value
Sequence of Vertex objects.
Exceptions
- An exception occurs if a feature with the given name does not exist.
Error : Incorrect feature name.
isAlignedWithSketch()
This method checks if the normal of an analytical rigid surface part is aligned with that of its sketch.
Arguments
None.
Return value
A Boolean value of True if the part is aligned with the sketch and False if it is not aligned.
Exceptions
- If the part is not an analytical rigid part:
AbaqusException: Can only be used with analytical rigid parts.
printAssignedSections()
This method prints information on each section that has been assigned to a region of the part.
Arguments
None.
Return value
None.
Exceptions
None.
projectEdgesOntoSketch(...)
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.
Required arguments
- sketch
The ConstrainedSketch object on which the edges are projected.
- edges
A sequence of candidate edges to be projected onto the sketch.
Optional arguments
- constrainToBackground
A Boolean that determines whether the projected edges need to constrained to the background geometry. The default is True.
Return value
None.
Exceptions
None.
projectReferencesOntoSketch(...)
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.
Required arguments
- sketch
The ConstrainedSketch object on which the edges, vertices, and datum points are projected.
Optional arguments
- filter
A SymbolicConstant specifying how to limit the amount of projection. Possible values are ALL_EDGES and COPLANAR_EDGES. If filter=COPLANAR_EDGES, edges that are coplanar to the sketching plane are the only candidates for projection. The default value is ALL_EDGES.
- upToFeature
A Feature object specifying a marker in the feature-based history of the part. Abaqus/CAE projects onto the sketch only the part entities that were created before the feature specified by this marker. By default, part entities in features created before the sketch you are editing are candidates for projection.
- edges
A sequence of candidate edges whose vertices need to be projected onto the sketch. By default, all edges specified by the filter argument are candidates for projection.
- vertices
A sequence of candidate vertices to be projected onto the sketch. By default, all vertices are candidates for projection.
Return value
None.
Exceptions
None.
queryAttributes(...)
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.
Required arguments
None.
Optional arguments
- printResults
A Boolean which specifies whether the above information is to be printed. The default value is True
Return value
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.
Exceptions
None.
queryCachedStates()
This method displays the position of geometric states relative to the sequence of features in the part cache. The output is displayed in the message area.
Arguments
None.
Return value
None.
Exceptions
None.
queryGeometry(...)
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).
Required arguments
None.
Optional arguments
- relativeAccuracy
A Float specifying that the property computations should stop when the specified relative accuracy has been achieved. The default value is 0.000001 (0.0001%).
- printResults
A Boolean which specifies whether the above information is to be printed. The default value is True.
Return value
A Dictionary object with string keys, which returns the above information with the keys being name, space, type, volume, centroid, category and boundingBox.
Exceptions
None.
queryRegionsMissingSections()
This method returns all regions in the part that do not have a section assignment but require one for analysis.
Arguments
None.
Return value
A Region object, or None.
Exceptions
None.
queryDisjointPlyRegions()
This method provides a list of all composite plys in the current part which have disjoint regions.
Arguments
None.
Return value
None.
Exceptions
None.
regenerate()
This method regenerates a part. When you modify features, it may be convenient to postpone regeneration until you make all your changes, since regeneration can be time consuming.
Arguments
None.
Return value
None.
Exceptions
None.
regenerationWarnings()
This method prints any regeneration warnings associated with the features.
Arguments
None.
Return value
None.
Exceptions
None.
removeInvalidGeometry()
Removes all invalid entities from the part, leaving a valid part. This is not recorded as a feature in the feature list, therefore it should be used on parts that have a single feature (such as an imported part).
Note:
This may remove valid entities that are connected to invalid ones. You can identify invalid entities using the query toolset before using this command.
Arguments
None.
Return value
None.
Exceptions
None.
restore()
This method restores the parameters of all features in the assembly to the value they had before a failed regeneration. Use the restore method after a failed regeneration, followed by a regenerate command.
Arguments
None.
Return value
None.
Exceptions
None.
resumeAllFeatures()
This method resumes all the suppressed features in the part.
Arguments
None.
Return value
None.
Exceptions
None.
resumeFeatures(...)
This method resumes the specified suppressed features in the part.
Required arguments
- featureNames
A tuple of names of features which are to be resumed.
Optional arguments
None.
Return value
None.
Exceptions
None.
resumeLastSetFeatures()
This method resumes the last set of features to be suppressed in the part.
Arguments
None.
Return value
None.
Exceptions
None.
saveGeometryCache()
This method caches the current geometry. Caching the current geometry improves regeneration performance.
Arguments
None.
Return value
None.
Exceptions
None.
setAssociatedCADPaths(...)
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.
Required arguments
None.
Optional arguments
- partFile
A String specifying the name of the associated CAD part file.
- rootFile
A String specifying the name of the root associated CAD file. This can be the same as the part file or can be the assembly file, depending on the one that was imported.
Return value
None.
Exceptions
None.
suppressFeatures(...)
This method suppresses the given features.
Required arguments
- featureNames
A tuple of names of features which are to be suppressed in the part.
Optional arguments
None.
Return value
None.
Exceptions
None.
writeAcisFile(...)
This method exports the geometry of the part to a named file in ACIS format.
Required arguments
- fileName
A String specifying the name of the file to which to write.
Optional arguments
- version
A Float specifying the ACIS version. For example, the Float 12.0 corresponds to ACIS Version 12.0. The default value is the current version of ACIS.
Return value
None.
Exceptions
- If the part is an orphan mesh part:
Cannot export orphan mesh parts to ACIS.
writeCADParameters(...)
This method writes the parameters that were imported from the CAD system to a parameter file.
Required arguments
- paramFile
A String specifying the parameter file name.
Optional arguments
- 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.
Return value
None.
Exceptions
None.
writeIgesFile(...)
This method exports the geometry of the part to a named file in IGES format.
Required arguments
- fileName
A String specifying the name of the file to which to write.
- flavor
A SymbolicConstant specifying a particular flavor of IGES. Possible values are STANDARD, AUTOCAD, SOLIDWORKS, JAMA, and MSBO.
Optional arguments
None.
Return value
None.
Exceptions
- If the part is an orphan mesh part:
Cannot export orphan mesh parts to IGES.
writeStepFile(...)
This method exports the geometry of the part to a named file in STEP format.
Required arguments
- fileName
A String specifying the name of the file to which to write.
Optional arguments
None.
Return value
None.
Exceptions
- If the part contains no geometry:
Parterror: Cannot export orphan mesh parts to STEP.
writeVdaFile(...)
This method exports the geometry of the part to a named file in VDA-FS format.
Required arguments
- fileName
A String specifying the name of the file to which to write.
Optional arguments
None.
Return value
None.
Exceptions
- If the part is an orphan mesh part:
Cannot export orphan mesh parts to VDA-FS.
copyMeshPattern(...)
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.
Required arguments
None.
Optional arguments
- 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.
Return value
None.
Exceptions
None.
smoothNodes(...)
This method smoothes the given nodes of a native mesh, moving them locally to a more optimal location that improves quality of the mesh
Required arguments
None.
Optional arguments
- nodes
A sequence of MeshNode objects or a Set object containing nodes. Nodes that are not part of native mesh only will be smoothed
- coordinates
A sequence of MeshNode objects or a Set object containing nodes.
Return value
None.
Exceptions
None.
Lock()
This method locks the part. Locking the part prevents any further changes to the part that can trigger regeneration of the part.
Arguments
None.
Return value
None.
Exceptions
None.
Unlock()
This method unlocks the part. Unlocking the part allows it to be regenerated after any modifications to the part.
Arguments
None.
Return value
None.
Exceptions
None.
LockForUpgrade()
This method locks the part for upgrade. Locking the part prevents any further changes to the part that can trigger regeneration of the part. When the part is unlocked, all the parts are upgraded and regenrated.
Arguments
None.
Return value
None.
Exceptions
None.
Members
The Part object has members with the same names and descriptions as the arguments to the Part method.
In addition, the Part object can have the following members:
- geometryValidity
A Boolean specifying the validity of the geometry of the part. The value is computed, but it can be set to ON to perform feature and mesh operations on an invalid part. There is no guarantee that such operations will work if the part was originally invalid.
- isOutOfDate
An Int specifying that feature parameters have been modified but that the part has not been regenerated. Possible values are 0 and 1.
- timeStamp
A Float specifying when the part was last modified.
- vertices
A VertexArray object specifying all the vertices in the part.
- ignoredVertices
An IgnoredVertexArray object specifying all the ignored vertices in the part.
- edges
An EdgeArray object specifying all the edges in the part.
- ignoredEdges
An IgnoredEdgeArray object specifying all the ignored edges in the part.
- faces
A FaceArray object specifying all the faces in the part.
- cells
A CellArray object specifying all the cells in the part.
- features
A repository of Feature objects specifying all the features in the part.
- featuresById
A repository of Feature objects specifying all Feature objects in the part. The Feature objects in the featuresById repository are the same as the Feature objects in the features repository. However, the key to the objects in the featuresById repository is an integer specifying the ID, whereas the key to the objects in the features repository is a string specifying the name.
- datums
A repository of Datum objects specifying all the datums in the part.
- elements
A MeshElementArray object specifying all the elements in the part.
- elemFaces
A repository of MeshFace objects specifying all the element faces in the part. For a given element and a given face index within that element, the corresponding MeshFace object can be retrieved from the repository by using the key calculated as (i*8 + j), where i and j are zero-based element and face indices, respectively.
- elementFaces
A MeshFaceArray object specifying all the unique element faces in the part.
- nodes
A MeshNodeArray object specifying all the nodes in the part.
- retainedNodes
A MeshNodeArray object specifying all the retained nodes in the substructure part.
- sets
A repository of Set objects specifying for more information, see Set.
- allSets
A repository of Set objects specifying the contents of the allSets repository is the same as the contents of the sets repository.
- allInternalSets
A repository of Set objects specifying picked regions.
- surfaces
A repository of Surface objects specifying for more information, see Surface.
- allSurfaces
A repository of Surface objects specifying the contents of the allSurfaces repository is the same as the contents of the surfaces repository.
- allInternalSurfaces
A repository of Surface objects specifying picked regions.
- skins
A repository of Skin objects specifying the skins created on the part.
- stringers
A repository of Stringer objects specifying the stringers created on the part.
- referencePoints
A repository of ReferencePoint objects.
- engineeringFeatures
An EngineeringFeature object.
- sectionAssignments
A SectionAssignmentArray object.
- materialOrientations
A MaterialOrientationArray object.
- compositeLayups
A repository of CompositeLayup objects.
- elemEdges
A repository of MeshEdge objects specifying all the element edges in the part. 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.
- elementEdges
A MeshEdgeArray object specifying all the unique element edges in the part.