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Part
Stephen S. Mitchell edited this page Apr 25, 2026
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Namespace: AlibreScript.API | Kind: Class
The Part class provides comprehensive functionality for creating, manipulating, and managing individual parts within Alibre Design. This class handles part properties, geometry creation, sketching, and file operations.
Parts are the foundation of mechanical design. Common scripting applications include:
- Automated part generation from design parameters
- Parametric modeling with configurable dimensions
- Feature creation (extrudes, cuts, fillets, chamfers)
- Sketch-based geometry for complex shapes
- Part validation and property management
- Batch operations on multiple parts
# Create a new part
part = Part("MyPart.AD_PRT", "C:\\MyProject")
# Add a sketch for the base feature
base_sketch = part.AddSketch("BaseSketch", part.GetPlane("XY"))
# Create geometry in the sketch
base_sketch.AddRectangle(0, 0, 50, 30, False)
base_sketch.AddCircle(25, 15, 5, False) # Center hole
# Create an extrude feature
part.AddExtrudeBoss(
"BaseExtrude", # Feature name
base_sketch, # Sketch to extrude
10.0, # Extrude distance
Part.EndCondition.Blind, # End condition
0.0, # Taper angle
False # Not thin wall
)
# Add a fillet to edges
part.AddFillet("EdgeFillet", ["Edge1", "Edge2"], 2.0)
# Save the part
part.Save("Part creation complete")- Assembly - Contains parts as components
- AssembledPart - Part within an assembly context
- Feature - Part features and operations
- Configuration - Part configurations
- GlobalParameters - Part parameters
- Properties - Part properties and metadata
- Methods - Available operations
- Sketching Methods - Drawing and sketching
- Feature Methods - Feature operations
- File Operations - Save, export, import
Type: Object
Comment property
Type: Object
List of configurations defined on the part
Type: Object
Cost center property
Type: Object
Created By property
Type: Object
Created Date property
Type: Object
Creating Application property
Type: Object
Density of the part
Type: Object
Description of the part
Type: Object
Document Number property
Type: Object
Engineering Approval Date property
Type: Object
Engineering Approved By property
Type: Object
Estimated Cost property
Type: Object
Material (extended information) property
Type: Object
Path and filename of the part
Type: Object
Keywords property
Type: Object
Last Author property
Type: Object
Last Update Date property
Type: Object
Manufacturing Approved By property
Type: Object
Product property
Type: Object
Mass of the part
Type: Object
Material of the part
Type: Object
Modified Information property
Type: Object
Name of the part
Type: Object
User-defined number for the part
Type: Object
Gets the origin (language independent)
Type: Object
List of parameters defined on the part
Type: Object
Product property
Type: Object
Received From property
Type: Object
Revision property
Type: Object
Gets the currently selected items as [ItemA, ItemB, ...]
Supports faces, edges, vertices, planes, axes and points
Type: Object
Stock Size property
Type: Object
Supplier property
Type: Object
Title property
Type: Object
Vendor property
Type: Object
Web Link property
Type: Object
Gets the X-axis (language independent)
Type: Object
Gets the XY-plane (language independent)
Type: Object
Gets the Y-axis (language independent)
Type: Object
Gets the YZ-plane (language independent)
Type: Object
Gets the Z-axis (language independent)
Type: Object
Gets the ZX-plane (language independent)
Opens an existing part
Overload 1:
def Part(folder, name):
"""
Opens an existing part
Args:
folder (str): Folder containing part
name (str): Name of part to open
"""Overload 2:
def Part(folder, name, hide_editor):
"""
Opens an existing part, optionally hiding the editor
Args:
folder (str): Folder containing part
name (str): Name of part to open
hide_editor (bool): True to hide the editor (only valid if part is not already open)
"""Overload 3:
def Part(name):
"""
Creates a new part
Args:
name (str): Name of new part
"""Overload 4:
def Part(name, create_new):
"""
Creates a new part or accesses an already opened part
Args:
name (str): Name of part to create or access
create_new (bool): True to create a new part, false to access an opened part
"""Overload 5:
def Part(name, create_new, hide_editor):
"""
Creates a new part or accesses an already opened part, optionally hiding the editor
Args:
name (str): Name of part to create or access
create_new (bool): True to create a new part, false to access an opened part
hide_editor (bool): True to hide the editor (only valid if CreateNew is true)
"""Overload 6:
def Part(file_name, type):
"""
Opens or imports an existing file for editing
Args:
file_name (str): Name of file to open
type (Part.FileTypes): Type of file (GeomagicDesignPart, STEP, IGES, ThreeDM, SAT, STL_in, STL_cm, STL_mm)
"""Overload 7:
def Part(file_name, type, hide_editor):
"""
Opens or imports an existing file for editing, optionally hiding the editor
Args:
file_name (str): Name of file to open
type (Part.FileTypes): Type of file (GeomagicDesignPart, STEP, IGES, ThreeDM, SAT, STL_in, STL_cm, STL_mm)
hide_editor (bool): True to hide the editor
"""Creates a new 3D sketch
def Add3DSketch(name):
"""
Creates a new 3D sketch
Args:
name (str): Name of sketch
Returns:
Created sketch
"""Creates an axis based on the intersection of two planes/faces
Overload 1:
def AddAxis(name, plane1, plane2):
"""
Creates an axis based on the intersection of two planes/faces
Args:
name (str): Name of axis
plane1 (ISketchSurface): First plane/face
plane2 (ISketchSurface): Second plane/face
Returns:
New Axis
"""Overload 2:
def AddAxis(name, point_a, point_b):
"""
Creates an axis based on two points
Args:
name (str): Name of axis
point_a (Point): First point object
point_b (Point): Second point object
Returns:
New axis
"""Overload 3:
def AddAxis(name, cylindrical_face):
"""
Creates an axis for a cylindrical face
Args:
name (str): Name of axis
cylindrical_face (Face): Cylindrical face
Returns:
New axis
"""Overload 4:
def AddAxis(name, point1, point2):
"""
Creates an axis based on two points
Args:
name (str): Name of axis
point1 (list): First point [X, Y, Z]
point2 (list): Second point [X, Y, Z]
Returns:
New axis
"""Adds a chamfer to a face or edge
Overload 1:
def AddChamfer(name, item, distance1, distance2, tangent_propagate):
"""
Adds a chamfer to a face or edge
Args:
name (str): Name of chamfer
item (IChamferable): Face or edge to chamfer
distance1 (float): First chamfer distance
distance2 (float): Second chamfer distance
tangent_propagate (bool): True to propagate the chamfer along connected edges
Returns:
Chamfer feature
"""Overload 2:
def AddChamfer(name, items, distance1, distance2, tangent_propagate):
"""
Adds a chamfer to a set of faces and edges
Args:
name (str): Name of chamfer
items (list): Faces and edges to chamfer
distance1 (float): First chamfer distance
distance2 (float): Second chamfer distance
tangent_propagate (bool): True to propagate the chamfer along connected edges
Returns:
Chamfer feature
"""Overload 3:
def AddChamfer(name, item, distance, tangent_propagate):
"""
Adds a chamfer to a face or edge
Args:
name (str): Name of chamfer
item (IChamferable): Face or edge to chamfer
distance (float): Chamfer distance
tangent_propagate (bool): True to propagate the chamfer along connected edges
Returns:
Chamfer feature
"""Overload 4:
def AddChamfer(name, items, distance, tangent_propagate):
"""
Adds a chamfer to a set of faces and edges
Args:
name (str): Name of chamfer
items (list): Faces and edges to chamfer
distance (float): Chamfer distance
tangent_propagate (bool): True to propagate the chamfer along connected edges
Returns:
Chamfer feature
"""Adds a chamfer to a face or edge
Overload 1:
def AddChamferAngle(name, item, distance, angle, tangent_propagate):
"""
Adds a chamfer to a face or edge
Args:
name (str): Name of chamfer
item (IChamferable): Face or edge to chamfer
distance (float): Chamfer distance
angle (float): Chamfer angle
tangent_propagate (bool): True to propagate the chamfer along connected edges
Returns:
Chamfer feature
"""Overload 2:
def AddChamferAngle(name, items, distance, angle, tangent_propagate):
"""
Adds a chamfer to a set of faces and edges
Args:
name (str): Name of chamfer
items (list): Faces and edges to chamfer
distance (float): Chamfer distance
angle (float): Chamfer angle
tangent_propagate (bool): True to propagate the chamfer along connected edges
Returns:
Chamfer feature
"""Adds a configuration to the part
Overload 1:
def AddConfiguration(name):
"""
Adds a configuration to the part
Args:
name (str): Name of configuration
Returns:
New configuration
"""Overload 2:
def AddConfiguration(name, base_configuration_name):
"""
Adds a configuration to the part using another configuration as a base
Args:
name (str): Name of configuration
base_configuration_name (str): Name of base configuration to use
Returns:
New configuration
"""Adds a simple extrude boss to a specific depth
Overload 1:
def AddExtrudeBoss(name, sketch, depth, is_reversed):
"""
Adds a simple extrude boss to a specific depth
Args:
name (str): Name of extrusion
sketch (Sketch): Sketch to extrude
depth (float): Extrusion distance
is_reversed (bool): True if extrusion direction is reversed
Returns:
Extruded feature
"""Overload 2:
def AddExtrudeBoss(name, sketch, depth, is_reversed, end_condition, end_plane, end_offset, direction, sweep_path, draft_angle, outward_draft):
"""
Adds an extrude feature
Args:
name (str): Name of extrusion
sketch (Sketch): Sketch to extrude
depth (float): Depth of extrusion
is_reversed (bool): true if direction is reversed
end_condition (Part.EndCondition): End condition for extrusion
end_plane (ISketchSurface): Face or plane to terminate extrusion
end_offset (float): Offset from face or plane to terminate extrusion
direction (Part.DirectionType): Direction of extrusion
sweep_path (ISweepPath): Sketch or edge to follow when extruding
draft_angle (float): Angle of draft
outward_draft (bool): true if outward draft
Returns:
Extruded feature
"""Adds a simple extrude cut to a specific depth
Overload 1:
def AddExtrudeCut(name, sketch, depth, is_reversed):
"""
Adds a simple extrude cut to a specific depth
Args:
name (str): Name of extrusion
sketch (Sketch): Sketch to extrude
depth (float): Extrusion distance
is_reversed (bool): True if extrusion direction is reversed
Returns:
Extruded feature
"""Overload 2:
def AddExtrudeCut(name, sketch, depth, is_reversed, end_condition, end_plane, end_offset, direction, sweep_path, draft_angle, outward_draft):
"""
Adds an extrude cut feature
Args:
name (str): Name of extrusion
sketch (Sketch): Sketch to extrude
depth (float): Depth of extrusion
is_reversed (bool): true if direction is reversed
end_condition (Part.EndCondition): End condition for extrusion
end_plane (ISketchSurface): Face or plane to terminate extrusion
end_offset (float): Offset from face or plane to terminate extrusion
direction (Part.DirectionType): Direction of extrusion
sweep_path (ISweepPath): Sketch or edge to follow when extruding
draft_angle (float): Angle of draft
outward_draft (bool): true if outward draft
Returns:
Extruded feature
"""Adds a constant radius fillet to a face or edge
Overload 1:
def AddFillet(name, item, radius, tangent_propagate):
"""
Adds a constant radius fillet to a face or edge
Args:
name (str): Name of fillet
item (IFilletable): Face or edge to fillet
radius (float): Radius of fillet
tangent_propagate (bool): True to propagate the fillet along connected edges
Returns:
Fillet feature
"""Overload 2:
def AddFillet(name, items, radius, tangent_propagate):
"""
Adds a constant radius fillet to a set of faces and edges
Args:
name (str): Name of fillet
items (list): Faces and edges to fillet
radius (float): Radius of fillet
tangent_propagate (bool): True to propagate the fillet along connected edges
Returns:
Fillet feature
"""Overload 3:
def AddFillet(name, items, start_radii, end_radii, tangent_propagate):
"""
Adds a variable radius fillet to a set of faces and edges
Args:
name (str): Name of fillet
items (list): Faces and edges to fillet
start_radii (list): Start radii of fillets
end_radii (list): End radii of fillets
tangent_propagate (bool): True to propagate the fillet along connected edges
Returns:
Fillet feature
"""Adds a gear sketch to the part
def AddGear(name, numberof_teeth, pitch_diameter, pressure_angle, diametral_pitch, single_tooth, center_x, center_y, involute_points, plane):
"""
Adds a gear sketch to the part
Args:
name (str): Name of gear sketch
numberof_teeth (float): Number of teeth
pitch_diameter (int): Diameter of pitch circle in current units
pressure_angle (float): Pressure angle (14.5 is typical)
diametral_pitch (float): Diametral angle (tooth size) (25.4/module) in teeth per inch
single_tooth (bool): true to create only a single tooth profile
center_x (float): X-coordinate of gear center
center_y (float): Y-coordinate of gear center
involute_points (int): Number of points for involute curve. Decreasing this makes Cubify/Geomagic faster. Increasing makes tooth profiles more accurate and allows gears with more teeth to be generated.
plane (ISketchSurface): Plane or face to create gear sketch on
Returns:
Gear sketch
"""Adds a gear sketch to the part using diametral pitch and number of teeth
Overload 1:
def AddGearDN(name, numberof_teeth, pressure_angle, diametral_pitch, center_x, center_y, plane):
"""
Adds a gear sketch to the part using diametral pitch and number of teeth
Args:
name (str): Name of gear sketch
numberof_teeth (float): Number of teeth
pressure_angle (int): Pressure angle (14.5 is typical)
diametral_pitch (float): Diametral angle (tooth size) (1/module)
center_x (float): X-coordinate of center of gear
center_y (float): Y-coordinate of center of gear
plane (ISketchSurface): Plane or face to create gear sketch on
Returns:
Gear sketch
"""Overload 2:
def AddGearDN(name, numberof_teeth, pressure_angle, diametral_pitch, center_x, center_y, single_tooth, plane):
"""
Adds a gear sketch to the part using diametral pitch and number of teeth
Args:
name (str): Name of gear sketch
numberof_teeth (float): Number of teeth
pressure_angle (int): Pressure angle (14.5 is typical)
diametral_pitch (float): Diametral angle (tooth size) (1/module)
center_x (float): X-coordinate of center of gear
center_y (float): Y-coordinate of center of gear
single_tooth (bool): True to generate a single tooth
plane (ISketchSurface): Plane or face to create gear sketch on
Returns:
Gear sketch
"""Adds a gear sketch to the part using diametral pitch and pitch diameter
Overload 1:
def AddGearDP(name, pitch_diameter, pressure_angle, diametral_pitch, center_x, center_y, plane):
"""
Adds a gear sketch to the part using diametral pitch and pitch diameter
Args:
name (str): Name of gear sketch
pitch_diameter (float): Diameter of pitch circle
pressure_angle (float): Pressure angle (14.5 is typical)
diametral_pitch (float): Diametral angle (tooth size) (1/module)
center_x (float): X-coordinate of center of gear
center_y (float): Y-coordinate of center of gear
plane (ISketchSurface): Plane or face to create gear sketch on
Returns:
Gear sketch
"""Overload 2:
def AddGearDP(name, pitch_diameter, pressure_angle, diametral_pitch, center_x, center_y, single_tooth, plane):
"""
Adds a gear sketch to the part using diametral pitch and pitch diameter
Args:
name (str): Name of gear sketch
pitch_diameter (float): Diameter of pitch circle
pressure_angle (float): Pressure angle (14.5 is typical)
diametral_pitch (float): Diametral angle (tooth size) (1/module)
center_x (float): X-coordinate of center of gear
center_y (float): Y-coordinate of center of gear
single_tooth (bool): True to generate a single tooth
plane (ISketchSurface): Plane or face to create gear sketch on
Returns:
Gear sketch
"""Adds a gear sketch to the part using number of teeth and pitch diameter
Overload 1:
def AddGearNP(name, numberof_teeth, pitch_diameter, pressure_angle, center_x, center_y, plane):
"""
Adds a gear sketch to the part using number of teeth and pitch diameter
Args:
name (str): Name of gear sketch
numberof_teeth (int): Number of teeth
pitch_diameter (float): Diameter of pitch circle
pressure_angle (float): Pressure angle (14.5 is typical)
center_x (float): X-coordinate of center of gear
center_y (float): Y-coordinate of center of gear
plane (ISketchSurface): Plane or face to create gear sketch on
Returns:
Gear sketch
"""Overload 2:
def AddGearNP(name, numberof_teeth, pitch_diameter, pressure_angle, center_x, center_y, single_tooth, plane):
"""
Adds a gear sketch to the part using number of teeth and pitch diameter
Args:
name (str): Name of gear sketch
numberof_teeth (int): Number of teeth
pitch_diameter (float): Diameter of pitch circle
pressure_angle (float): Pressure angle (14.5 is typical)
center_x (float): X-coordinate of center of gear
center_y (float): Y-coordinate of center of gear
single_tooth (bool): True to generate a single tooth
plane (ISketchSurface): Plane or face to create gear sketch on
Returns:
Gear sketch
"""Adds a loft extrusion
Overload 1:
def AddLoftBoss(name, cross_sections, minimize_twist, minimize_curvature, simplify_surface, connect_ends):
"""
Adds a loft extrusion
Args:
name (str): Name of loft
cross_sections (list): Python list of cross sections (faces, 2D sketches, design points)
minimize_twist (bool): True to minimize twist
minimize_curvature (bool): True to minimize curvature
simplify_surface (bool): True to simplify the loft surface
connect_ends (bool): True to connect the start of the loft with the end
Returns:
Extruded feature
"""Overload 2:
def AddLoftBoss(name, cross_sections, guide_curves, guide_type, minimize_twist, minimize_curvature, simplify_surface, connect_ends):
"""
Adds a loft extrusion using guide curves
Args:
name (str): Name of loft
cross_sections (list): Python list of cross sections (faces, 2D sketches, design points)
guide_curves (list): Python list of guide curves (3D sketches)
guide_type (GuideCurveTypes): Type of guide curve
minimize_twist (bool): True to minimize twist
minimize_curvature (bool): True to minimize curvature
simplify_surface (bool): True to simplify the loft surface
connect_ends (bool): True to connect the start of the loft with the end
Returns:
Extruded feature
"""Adds a loft cut
Overload 1:
def AddLoftCut(name, cross_sections, minimize_twist, minimize_curvature, simplify_surface, connect_ends):
"""
Adds a loft cut
Args:
name (str): Name of loft
cross_sections (list): Python list of cross sections (faces, 2D sketches, design points)
minimize_twist (bool): True to minimize twist
minimize_curvature (bool): True to minimize curvature
simplify_surface (bool): True to simplify the loft surface
connect_ends (bool): True to connect the start of the loft with the end
Returns:
Cut feature
"""Overload 2:
def AddLoftCut(name, cross_sections, guide_curves, guide_type, minimize_twist, minimize_curvature, simplify_surface, connect_ends):
"""
Adds a loft cut using guide curves
Args:
name (str): Name of loft
cross_sections (list): Python list of cross sections (faces, 2D sketches, design points)
guide_curves (list): Python list of guide curves (3D sketches)
guide_type (GuideCurveTypes): Type of guide curve
minimize_twist (bool): True to minimize twist
minimize_curvature (bool): True to minimize curvature
simplify_surface (bool): True to simplify the loft surface
connect_ends (bool): True to connect the start of the loft with the end
Returns:
Extruded feature
"""Adds a cm/mm/in/deg parameter to the part
Overload 1:
def AddParameter(name, type, value):
"""
Adds a cm/mm/in/deg parameter to the part
Args:
name (str): Name of parameter
type (ParameterTypes): Type of parameter
value (float): Value for parameter
Returns:
New parameter
"""Overload 2:
def AddParameter(name, type, unitsto_use, value):
"""
Adds a parameter to the part with specific units
Args:
name (str): Name of parameter
type (ParameterTypes): Type of parameter
unitsto_use (ParameterUnits): Units to use
value (float): Value for parameter
Returns:
New parameter
"""Overload 3:
def AddParameter(name, type, equation):
"""
Adds a parameter to the part
Args:
name (str): Name of parameter
type (ParameterTypes): Type of parameter
equation (str): Equation for parameter
Returns:
New parameter
"""Creates a plane based on the offset from an existing plane
Overload 1:
def AddPlane(name, source_plane, offset):
"""
Creates a plane based on the offset from an existing plane
Args:
name (str): Name of plane
source_plane (ISketchSurface): Plane/face to use as basis
offset (float): Offset from basis plane in currently chosen units
Returns:
Created plane
"""Overload 2:
def AddPlane(name, normal_vector, pointon_plane):
"""
Adds a plane using a normal vector and a point on the plane
Args:
name (str): Name of plane to add
normal_vector (list): Normal vector as a list [nx, ny, nz]. Does not need to be a unit vector
pointon_plane (list): A point on the plane as a list [px, py, pz]
Returns:
Created plane
"""Overload 3:
def AddPlane(name, axis, point):
"""
Creates a new plane contaning an axis and a point
Args:
name (str): Name of new plane
axis (Axis): Axis that lies on plane
point (Point): Point that lies on plane
Returns:
New plane
"""Overload 4:
def AddPlane(name, source_plane, rotation_axis, angle):
"""
Creates a new plane at an angle to an existing plane
Args:
name (str): Name of new plane
source_plane (ISketchSurface): Plane/face to use as basis for new plane
rotation_axis (Axis): Axis of rotation for new plane
angle (float): Angle of new plane in degrees
Returns:
New plane
"""Overload 5:
def AddPlane(name, point1, point2, point3):
"""
Creates a plane using three points. Each point is defined as list of [x, y, z]
Args:
name (str): Name of plane
point1 (list): Point on plane
point2 (list): Point on plane
point3 (list): Point on plane
Returns:
Created plane
"""Adds a point to the part
Overload 1:
def AddPoint(name, point):
"""
Adds a point to the part
Args:
name (str): Name of the new point
point (list): Point location [x, y, z]
Returns:
The new point
"""Overload 2:
def AddPoint(name, point):
"""
Adds a point to the part
Args:
name (str): Name of the point
point (Point): Point to add
"""Overload 3:
def AddPoint(name, x, y, z):
"""
Adds a point to the part
Args:
name (str): Name of new point
x (float): X coordinate
y (float): Y coordinate
z (float): Z coordinate
Returns:
The new point
"""Overload 4:
def AddPoint(name, point_or_vertex, x_offset, y_offset, z_offset):
"""
Add a point at an offset to a point or a vertex
Args:
name (str): Name of point
point_or_vertex (IPoint): Point or vertex
x_offset (float): X offse
y_offset (float): Y offset
z_offset (float): Z offset
Returns:
The created point
"""Overload 5:
def AddPoint(name, point_or_vertex1, point_or_vertex2, ratio):
"""
Add a point between two points/vertices
Args:
name (str): Name of point
point_or_vertex1 (IPoint): First point or vertex
point_or_vertex2 (IPoint): Second point or vertex
ratio (float): Ratio of distance between points/vertices
Returns:
The created point
"""Overload 6:
def AddPoint(name, axis_or_edge1, axis_or_edge2):
"""
Add a point at the intersection or two axes or edges
Args:
name (str): Name of point
axis_or_edge1 (IAxis): First axis or edge
axis_or_edge2 (IAxis): Second axis or edge
Returns:
The created point
"""Overload 7:
def AddPoint(name, plane_or_face1, plane_or_face2, plane_or_face3):
"""
Add a point at the intersection of three planes or faces
Args:
name (str): Name of point
plane_or_face1 (IPlane): First plane or face
plane_or_face2 (IPlane): Second plane or face
plane_or_face3 (IPlane): Third plane or face
Returns:
The created point
"""Overload 8:
def AddPoint(name, axis_or_edge, plane_or_face):
"""
Add a point at the the intersection of a axis or edge and a plane or face
Args:
name (str): Name of point
axis_or_edge (IAxis): Axis or edge
plane_or_face (IPlane): Plane or face
Returns:
The created point
"""Overload 9:
def AddPoint(name, source_point_or_vertex, target_plane_or_face, x_offset, y_offset):
"""
Add a point by projecting a point or vertex onto a plane or face
Args:
name (str): Name of point
source_point_or_vertex (IPoint): Point or vertex to project
target_plane_or_face (IPlane): Plane or face to project onto
x_offset (float): X offset to apply to point once projected
y_offset (float): Y offset to apply to point once projected
Returns:
The created point
"""Overload 10:
def AddPoint(name, target_edge, ratio):
"""
Add a point on an edge
Args:
name (str): Name of point
target_edge (Edge): The edge to create the point on
ratio (float): Ratio along the edge from 0.0 -> 1.0
Returns:
The created point
"""Adds a point at the center of a circular edge
def AddPointFromCircularEdge(name, target_edge):
"""
Adds a point at the center of a circular edge
Args:
name (str): Name of point
target_edge (Edge): The edge to use for creating the point
Returns:
The created point
"""Adds a point at the center of a toroidal face
def AddPointFromToroidalFace(name, target_face):
"""
Adds a point at the center of a toroidal face
Args:
name (str): Name of point
target_face (Face): Toroidal face to use in creating the point
Returns:
The created point
"""Adds a set of points to the part
def AddPoints(prefix, points):
"""
Adds a set of points to the part
Args:
prefix (str): Prefix for the point names
points (list): List of points [x1,y1,z1, ..., xn,yn,zn]
"""Creates a revolve boss feature
def AddRevolveBoss(name, sketch, axis, angle):
"""
Creates a revolve boss feature
Args:
name (str): Name of feature
sketch (Sketch): Sketch to revolve
axis (Axis): Axis to rotate around
angle (float): Rotation angle in degrees
Returns:
Created feature
"""Creates a revolve cut feature
def AddRevolveCut(name, sketch, axis, angle):
"""
Creates a revolve cut feature
Args:
name (str): Name of feature
sketch (Sketch): Sketch to revolve
axis (Axis): Axis to rotate around
angle (float): Rotation angle in degrees
Returns:
Created feature
"""Creates a new sketch using a plane/face
def AddSketch(name, plane):
"""
Creates a new sketch using a plane/face
Args:
name (str): Name of sketch
plane (ISketchSurface): Plane/face to use for sketch
Returns:
Created sketch
"""Adds a sweep extrude feature
def AddSweepBoss(name, profile_sketch, path_sketch, is_rigid, end_condition, end_plane, end_offset, draft_angle, outward_draft):
"""
Adds a sweep extrude feature
Args:
name (str): Name of extrusion
profile_sketch (Sketch): Sketch to extrude
path_sketch (ISweepPath): Sketch or edge to sweep along
is_rigid (bool): true if path is parallel to profile
end_condition (Part.EndCondition): End condition for extrusion
end_plane (ISketchSurface): Face or plane to terminate extrusion
end_offset (float): Offset from face or plane to terminate extrusion
draft_angle (float): Angle of draft
outward_draft (bool): true if outward draft
Returns:
Extruded feature
"""Adds a sweep extrude cut feature
def AddSweepCut(name, profile_sketch, path_sketch, is_rigid, end_condition, end_plane, end_offset, draft_angle, outward_draft):
"""
Adds a sweep extrude cut feature
Args:
name (str): Name of extrusion
profile_sketch (Sketch): Sketch to extrude
path_sketch (ISweepPath): Sketch or edge to sweep along
is_rigid (bool): true if path is parallel to profile
end_condition (Part.EndCondition): End condition for extrusion
end_plane (ISketchSurface): Face or plane to terminate extrusion
end_offset (float): Offset from face or plane to terminate extrusion
draft_angle (float): Angle of draft
outward_draft (bool): true if outward draft
Returns:
Extruded feature
"""Adds a chamfer to a vertex
Overload 1:
def AddVertexChamfer(name, item, distance1, distance2, distance3):
"""
Adds a chamfer to a vertex
Args:
name (str): Name of chamfer
item (Vertex): Vertex to chamfer
distance1 (float): First chamfer distance
distance2 (float): Second chamfer distance
distance3 (float): Third chamfer distance
Returns:
Chamfer feature
"""Overload 2:
def AddVertexChamfer(name, items, distance1, distance2, distance3):
"""
Adds a chamfer to a set of vertices
Args:
name (str): Name of chamfer
items (list): Vertices to chamfer
distance1 (float): First chamfer distance
distance2 (float): Second chamfer distance
distance3 (float): Third chamfer distance
Returns:
Chamfer feature
"""Exports a keyshot file
def ExportBIP(file_name):
"""
Exports a keyshot file
Args:
file_name (str): Path and name of keyshot file
"""Exports the part as a IGES file
def ExportIGES(file_name):
"""
Exports the part as a IGES file
Args:
file_name (str): Path and name of IGES file
"""Exports the part as an STL rotated so that a specific face is on the bottom
def ExportRotatedSTL(file_name, bottom_face, forceto_millimeters, use_custom_settings, max_cell_size, normal_deviation, surface_deviation):
"""
Exports the part as an STL rotated so that a specific face is on the bottom
Args:
file_name (str): Path and name of STL file
bottom_face (Face): Face to use as bottom of part
forceto_millimeters (bool): true to output STL in millimeters regardless of part units
use_custom_settings (bool): true to use custom STL settings, false to use settings in system properties
max_cell_size (float): Custom max cell size
normal_deviation (float): Custom normal deviation
surface_deviation (float): Custom surface deviation
"""Exports the part as a SAT file
def ExportSAT(file_name, version, save_colors):
"""
Exports the part as a SAT file
Args:
file_name (str): Path and name of SAT file
version (int): Exported SAT file version
save_colors (bool): true to preseve colors
"""Exports the part as a STEP 203 file
def ExportSTEP203(file_name):
"""
Exports the part as a STEP 203 file
Args:
file_name (str): Path and name of STEP 203 file
"""Exports the part as a STEP 214 file
def ExportSTEP214(file_name):
"""
Exports the part as a STEP 214 file
Args:
file_name (str): Path and name of STEP 214 file
"""Exports the part as an STL file
def ExportSTL(file_name):
"""
Exports the part as an STL file
Args:
file_name (str): Path and name of STL file
"""Gets a sketch using the name of the sketch
def Get3DSketch(name):
"""
Gets a sketch using the name of the sketch
Args:
name (str): Name of sketch
Returns:
Sketch object
"""Gets an axis from an axis name
def GetAxis(name):
"""
Gets an axis from an axis name
Args:
name (str): Name of axis to find
Returns:
Found axis
"""Gets a configuration with a specific name
def GetConfiguration(name):
"""
Gets a configuration with a specific name
Args:
name (str): Name of confguration
Returns:
Configuration object
"""Gets the value of a custonm property
def GetCustomProperty(name):
"""
Gets the value of a custonm property
Args:
name (str): Name of the custom property
Returns:
The value of the property as a string
"""Gets an edge using it's name "Edge"
def GetEdge(name):
"""
Gets an edge using it's name "Edge<n>"
Args:
name (str): Name of edge
Returns:
Edge if found
"""Gets a face using it's name "Face"
def GetFace(name):
"""
Gets a face using it's name "Face<n>"
Args:
name (str): Name of face
Returns:
Face if found
"""Gets a feature on the part
def GetFeature(name):
"""
Gets a feature on the part
Args:
name (str): Name of the feature to get
Returns:
The feature or null if not found
"""Gets a parameter with a specific name
def GetParameter(name):
"""
Gets a parameter with a specific name
Args:
name (str): Name of parameter
Returns:
Parameter object
"""Gets a plane using the name of the plane
def GetPlane(name):
"""
Gets a plane using the name of the plane
Args:
name (str): Name of plane to find
Returns:
The plane
"""Gets a point on the part using the point name. The point must have been created in a script
def GetPoint(name):
"""
Gets a point on the part using the point name. The point must have been created in a script
Args:
name (str): Name of point to get
Returns:
Point on the part
"""Gets a sketch using the name of the sketch
def GetSketch(name):
"""
Gets a sketch using the name of the sketch
Args:
name (str): Name of sketch
Returns:
Sketch object
"""Gets user data
def GetUserData(name):
"""
Gets user data
Args:
name (str): Name of data to get
Returns:
Data as a python dictionary or None if not found
"""Gets a vertex using it's name "Vertex"
def GetVertex(name):
"""
Gets a vertex using it's name "Vertex<n>"
Args:
name (str): Name of vertex
Returns:
Vertex if found
"""Hides a feature on the part
Overload 1:
def HideFeature(name):
"""
Hides a feature on the part
Args:
name (str): Name of the feature to hide
"""Overload 2:
def HideFeature(feature):
"""
Hides a feature on the part
Args:
feature (Feature): Feature to hide
"""Non-uniform scaling of the part
def NonUniformScale(name, scale_about_center, scale_factor_x, scale_factor_y, scale_factor_z):
"""
Non-uniform scaling of the part
Args:
name (str): Name of the scaling
scale_about_center (bool): true to scale around the center of the part
scale_factor_x (float): X scale factor
scale_factor_y (float): Y scale factor
scale_factor_z (float): Z scale factor
Returns:
Scale feature
"""Removes a feature from the part
Overload 1:
def RemoveFeature(name):
"""
Removes a feature from the part
Args:
name (str): Name of the feature to remove
"""Overload 2:
def RemoveFeature(feature):
"""
Removes a feature from the part
Args:
feature (Feature): Feature to remove
"""Removes a plane from the part
def RemovePlane(plane):
"""
Removes a plane from the part
Args:
plane (Plane): Plane to remove
"""Removes a point from the part
def RemovePoint(point):
"""
Removes a point from the part
Args:
point (Point): Point to remove
"""Removes a sketch from the part
Overload 1:
def RemoveSketch(name):
"""
Removes a sketch from the part
Args:
name (str): Name of sketch to remove
"""Overload 2:
def RemoveSketch(sketch):
"""
Removes a sketch from the part
Args:
sketch (Sketch): Sketch to remove
"""Saves the part to a specific folder
def Save(folder):
"""
Saves the part to a specific folder
Args:
folder (str): Folder to save to
"""Saves the part to a specific folder with a new name
def SaveAs(folder, new_name):
"""
Saves the part to a specific folder with a new name
Args:
folder (str): Folder to save to
new_name (str): New name for part
"""Saves the current view as a bitmap image
def SaveSnapshot(file_name, width, height, use_aspect_ratio, use_widthand_height):
"""
Saves the current view as a bitmap image
Args:
file_name (str): Path and name of file to save to
width (int): Width in pixels
height (int): Height in pixels
use_aspect_ratio (bool): if true uses greater of width/height along with current aspect ratio
use_widthand_height (bool): if true uses current width/height of view
"""Saves a thumbnail image of the part
def SaveThumbnail(file_name, width, height):
"""
Saves a thumbnail image of the part
Args:
file_name (str): Path and name of file to save to
width (int): Width of thumbnail in pixels
height (int): Height of thumbnail in pixels
"""Uniform scaling of the part
def Scale(name, scale_about_center, scale_factor):
"""
Uniform scaling of the part
Args:
name (str): Name of the scaling
scale_about_center (bool): true to scale around the center of the part
scale_factor (float): Scale factor
Returns:
Scale feature
"""Selects a face, edge, vertex, point, axis, plane, sketch
Overload 1:
def Select(faceor_edge):
"""
Selects a face, edge, vertex, point, axis, plane, sketch
Args:
faceor_edge (ISelectableGeometry): Face, edge, vertex, point, axis plane or sketch to select
"""Overload 2:
def Select(faces_edges_list):
"""
Selects a group of faces, edges, vertices, points, axes, planes and sketches
Args:
faces_edges_list (list): List of Faces, edges, vertices, points, axes, planes and sketches to select [FaceA, FaceB, EdgeA, EdgeB, ...]
"""Sets the color of the part
def SetColor(red, green, blue):
"""
Sets the color of the part
Args:
red (byte): Red component 0 - 255
green (byte): Green component 0 - 255
blue (byte): Blue component 0 - 255
"""Sets the value of a custom property The custom property must already be defined on the part or defined on the user's PC
def SetCustomProperty(name, value):
"""
Sets the value of a custom property The custom property must already be defined on the part or defined on the user's PC
Args:
name (str): Name of the custom property
value (str): New value for the custom property
"""Sets user data
def SetUserData(name, dict):
"""
Sets user data
Args:
name (str): Data name of the format companyname.projectname.dataname
dict (IronPython.Runtime.PythonDictionary): Python dictionary of data to store
"""Shows a feature on the part
Overload 1:
def ShowFeature(name):
"""
Shows a feature on the part
Args:
name (str): Name of the feature to show
"""Overload 2:
def ShowFeature(feature):
"""
Shows a feature on the part
Args:
feature (Feature): Feature to show
"""Suppresses a feature on the part
Overload 1:
def SuppressFeature(name):
"""
Suppresses a feature on the part
Args:
name (str): Name of the feature to suppress
"""Overload 2:
def SuppressFeature(feature):
"""
Suppresses a feature on the part
Args:
feature (Feature): Feature to suppress
"""Unsuppresses a feature on the part
Overload 1:
def UnsuppressFeature(name):
"""
Unsuppresses a feature on the part
Args:
name (str): Name of the feature to unsuppress
"""Overload 2:
def UnsuppressFeature(feature):
"""
Unsuppresses a feature on the part
Args:
feature (Feature): Feature to unsuppress
"""Documentation Home | Classes | Methods Index | Properties Index | Members Index
Generated on 2025-09-23 02:06