Operations

• Reference
  • Plane (hwx.inspire.core)
  • Axis (hwx.inspire.core)
  • Point (hwx.inspire.core)

---

pushPull	extract	mirror
patch	rotate	translate
move	deleteFaces	scale
booleanCombine	booleanSubtract	booleanIntersect
slice	simplifyImprints	simplifyRounds
simplifyHoles	simplifyPlugs	partition
midSurface	chamferByAngle	chamferByDistance
shell	extrude	offset
thicken	linearPattern	createPipe
moveFaces	intersect	convertToMass
replaceFromFile	replaceFromPart	circularPattern
draft	convertBodiesToParts	breakInstance
projectAndSplit	revolve2	edgeFillet
sweep	nurbsCurve	patternAlongPath
multiSweep	loft	helixCurve
divideCurve

pushPull(feature, depth, newPart=False, resultType=None)

Pushes or pulls a face or an edge to a specified distance.

param feature

Feature to push or pull.

type feature

FeatureArea

param depth

The precise distance. A positive value extends, whereas a negative value contracts.

type depth

float | str

param newPart

If True, creates a new Part as a result of pushPull operation.

type newPart

bool

param resultType

Result type of pushPull operation. This option is valid only for pushPull a sketch on face. - NEW_PART - ADD - REMOVE - REPLACE

type resultType

str

returns

If New Part created, otherwise return None.

rtype

Part

extract(features, maintainReference=True)

Extracts geometry features and transfer them into a new part.

param features

Feature to be extracted.

type features

list[Feature]

param maintainReference

If true, set reference associativity otherwise not.

type maintainReference

bool

returns

New part created.

rtype

Part

mirror(entity, planeOrigin=None, planeNormal=None, keep=True)

Mirrors part across a symmetry plane.

If entity is a Part, the planeOrigin and planeNormal need to be passed

param entity

Part from which a mirror part needs to be created or a Planar feature which needs to be mirrored across the plane

type entity

Part | FeaturePlanar

param planeOrigin

The origin of the symmetry plane.

type planeOrigin

math.Point

param planeNormal

The normal of the symmetry plane.

type planeNormal

math.Vector

param keep

If True it keeps the original part, if False it removes it.

type keep

bool

returns

New mirrored part created.

rtype

Part

patch(features)

Creates patches to fill in specified missing surfaces.

param features

Features to be patched.

type features

list[Feature]

returns

New parts created.

rtype

list[Part]

rotate(part, axis, angle, degrees=True)

Rotates a part around the specified axis.

This is a body rotation.

param part

The part to rotate.

type part

Part

param axis

The rotation axis. If axis a string, valid choices are “x”, “y”, “z”.

type axis

Vector | str

param angle

The rotation angle.

type angle

float

param degrees

If True, angle is considered in degrees, if False in radians.

type degrees

bool

translate(part, x=0, y=None, z=None)

Translates by the specified distance.

If y is None, x is assumed to be a list of 3 floats.

param part

The part to translate.

type part

Part

param x

The distance to translate the ‘x’ vector.

type x

float

param y

The distance to translate the ‘y’ vector.

type y

float

param z

The distance to translate the ‘z’ vector.

type z

float

move(part, position)

Translates and/or rotates a part.

param part

The part to move.

type part

Part

param position

The position to move the part at.

type position

math.Matrix44

deleteFaces(features)

Deletes the specified faces from the part.

param features

Features to be removed.

type features

list[Feature]

scale(parts, value=1.1)

Resizes the part to the specified scale value.

This is useful when working with an imported model that is associated with a different default unit system.

param parts

Parts that need to be scaled.

type parts

list[Part]

param value

The scale factor. If value is a string it can be a Model Variable or a value with units.

type value

float | str

booleanCombine(target, tools=None)

Combines the specified parts.

param target

Part to be combined with tools.

type target

Part

param tools

Parts to be combined with target. Destroyed after combine.

type tools

list[Part]

returns

The combined part.

rtype

Part

booleanSubtract(targets, tools, keepTools=False)

Carves out one set of solid objects from another set of solid objects.

param targets

The parts being carved.

type targets

list[Part]

param tools

The parts doing the carving.

type tools

list[Part]

param keepTools

If True, preserves the tools after the operation.

type keepTools

bool

returns

The remaining part.

rtype

Part

booleanIntersect(targets, tools, keepTargets=False, keepTools=False)

Retains only the intersecting portions of two sets of solid objects.

param targets

The first set of parts.

type targets

list[Part]

param tools

A list of parts for boolean intersect operation.

type tools

list[Part]

param keepTargets

If True, preserves the target parts after the operation.

type keepTargets

bool

param keepTools

If True, preserves the tools parts after the operation.

type keepTools

bool

returns

The intersected part.

rtype

Part

slice(targets, cutOrigin=None, cutNormal=None, surfaceFeature=None, extendSurface=True)

Slices a set of solid objects with a cutting plane or cutting surface.

You must provide cutOrigin and cutNormal or surfaceFeature.

param targets

The parts to slice across the cutting plane.

type targets

list[Part]

param cutOrigin

The origin of the cutting plane.

type cutOrigin

math.Point

param cutNormal

The normal of the cutting plane.

type cutNormal

math.Vector

param surfaceFeature

The surface to slice the enity accross.

type surfaceFeature

FeatureArea

param extendSurface

Set Automatic extension On/Off for tool Surface.

type extendSurface

bool

returns

The new sliced part created.

rtype

Part

simplifyImprints(entity)

Finds and removes imprints from a part.

An imprint is an edge or a point that appears on a surface that can be removed without changing the underlying integrity of the surface, such as scratches or trimmed points.

param entity

Part/Assembly from which you want to remove the imprints from or FeatureLinear imprint to be removed.

type entity

Part | Assembly | FeatureLinear

simplifyRounds(entity, roundType='ALL', minSize=0, maxSize=None)

Finds and removes both round (convex) and fillet (concave) surfaces.

param entity

Part/Assembly from which you want to remove the fillets, chamfers from or a Feature to be removed.

type entity

Part | Assembly | Feature

param roundType

Valid values are: ROUNDS, FILLETS, CHAMFERS and ALL.

type roundType

str

param minSize

Minimum size of round.

type minSize

float

param maxSize

Maximum size of round.

type maxSize

float

simplifyHoles(entity, minSize=0, maxSize=None)

Finds and removes holes and pockets, and find raised areas such as lettering.

param entity

Part/Assembly from which you want to remove the holes from or FeatureCircular which needs to be removed.

type entity

Part | Assembly | Feature

param minSize

Minimum size of hole.

type minSize

float

param maxSize

Maximum size of hole.

type maxSize

float

simplifyPlugs(entity, minSize=0, maxSize=None)

Finds holes and pockets, and plug them by filling the area with a new part

param entity

Part/Assembly from which you want to plug the holes or a Circular feature that needs to be plugged.

type entity

Part | Assembly | Feature

param minSize

Minimum size of plug.

type minSize

float

param maxSize

Maximum size of plug.

type maxSize

float

partition(feature, thickness='1 mm', reverseDirection=False)

Divides a solid part into design and non-design regions by selecting a hole, pocket, or face to offset.

param feature

Feature to be partitioned.

type feature

Feature

param thickness

The partition thickness consider in mm.

type thickness

float

param reverseDirection

Switch the direction of the offset for the partition.

type reverseDirection

bool

returns

New part created.

rtype

Part

midSurface(part, surfaceOptions='Mid')

Extracts a midsurface or side faces from thin solids, and determine where surfaces are represented.

Replacing parts with midsurfaces yields better results while increasing speed when running an analysis or optimization.

param part

The part which needs midsurface extraction.

type part

Part

param surfaceOptions

This options allows you to extract the Mid, Left or Right surface of the part.

type surfaceOptions

str

chamferByAngle(feature, angle=45, dist=0.003)

Creates chamfer on a Linear/Planar feature.

param feature

Feature that needs to be chamfer.

type feature

Feature

param angle

Chamfer angle from the edge.

type angle

float

param dist

Chamfer distance from the edge.

type dist

float

chamferByDistance(feature, dist1=0.003, dist2=0.003)

Creates chamfer on a linear or planar feature.

param feature

Feature that needs to be chamfer.

type feature

Feature

param dist1

Chamfer distance from the edge.

type dist1

float

param dist2

Chamfer distance from the edge.

type dist2

float

shell(feature, thickness=1)

Removes material and create thin walls to generate a shelled part.

param feature

Feature to create a shelled part from.

type feature

FeatureArea

param thickness

Shell thickness.

type thickness

float

extrude(features, direction, resultType, parts=None, extrudeAsSolid=True, reference=None, extrudeTo1=1, extrudeTo2=1, angle1=0, angle2=0, extrusionEndCaps=None)

Extrude sketch profile.

param features

The features of the sketch to extrude.

type features

list[Feature]

param extrudeAsSolid

If True extrude as Solid, otherwise extrude as Sheet.

type extrudeAsSolid

bool

param direction

Valid directions to extrude are: SINGLE, BOTH and SYMMETRY.

type direction

str

param resultType

Valid choices are: COMBINE, SUBTRACT, INTERSECT and NEW_PART.

type resultType

str

param parts

Parts you would like to merge the extruded shape with. Defaults to None. That means the extruded shape will be merged with all parts that touch it.

type parts

list[Part]

param reference

Direction vector of extrusion. Defaults to the feature normal.

type reference

math.Vector | FeatureLinear | System

param extrudeTo1

If extrudeTo1 is a float then its the extrusion length in direction 1 in meters. If extrudeTo1 is a FeautrePoint or a FeaturePlanar then its used to determine the extrusion length in direction 1. If value is a string it can be a Model Variable or a value with units.

type extrudeTo1

float | FeaturePlanar | FeaturePoint | str

param extrudeTo2

If value is a float then it’s the extrusion length in direction 2 in meters. If value is a FeautrePoint or a FeaturePlanar then it’s used to determine the extrusion length in direction 2. If value is a string it can be a Model Variable or a value with units.

type extrudeTo2

float | FeaturePlanar | FeaturePoint | str

param angle1

The draft angle in direction 1 in degree. If value is a string it can be a Model Variable or a value with units.

type angle1

float | str

param angle2

The draft angle in direction 2 in degree. If value is a string it can be a Model Variable or a value with units.

type angle2

float | str

param extrusionEndCaps

Valid choices are: NONE, BOTH, START and END.

type extrusionEndCaps

str

returns

New part created.

rtype

Part

offset(input, value, newPart=False)

Offset surfaces or parts.

param input

type input

list[Part] | list[Feature]

param value

Desired offset distance. Negative value means inward direction. If value is a string it can be a Model Variable or a value with units.

type value

float | str

param newPart

If True, creates a new part.

type newPart

bool

returns

New part created if newPart was True.

rtype

Part|None

thicken(parts, value, symmetric=True)

Thicken surface parts and convert them to solids, or thicken and hollow solid parts.

When used on a solid part, the Thicken tool yields a hollow solid. When used on a surface part, the Thicken tool yields a solid part.

param parts

type parts

list[Part]

param value

Desired offset distance. Negative value means inward direction.

type value

float

param symmetric

If True, offsets symmetrically on both sides of the part surface.

type symmetric

bool

linearPattern(input, direction1, direction2=(0, 0, 0), bothDirection=False, spacing1=0.0, count1=3, spacing2=0.0, count2=3, instances=False, symmetry1=False, symmetry2=False, reverseDir1=False, reverseDir2=False, copiesToSkip=None, seedOnly=False)

Linear Pattern parts or faces along a direction.

param input

type input

list[Part]

param direction1

Direction can be a reference line, edge, or axis to which the pattern will be parallel.

type direction1

math.Vector | FeatureCurve | System

param direction2

Direction can be a reference line, edge, or axis to which the pattern will be parallel.

type direction2

math.Vector | FeatureCurve | System

param bothDirection

If True, sets in both direction otherwise single direction.

type bothDirection

bool

param spacing1

Distance between two copies.

type spacing1

float

param count1

Number of copies.

type count1

int

param spacing2

Distance between two copies.

type spacing2

float

param count2

Number of copies.

type count2

int

param instances

If True, any changes to part or face will apply to all instances.

type instances

bool

param symmetry1

Symmetry in Direction 1.

type symmetry1

bool

param symmetry2

Symmetry in Direction 2.

type symmetry2

bool

param reverseDir1

Reverse the pattern direction in Direction 1.

type reverseDir1

bool

param reverseDir2

Reverse the pattern direction in Direction 2.

type reverseDir2

bool

param copiesToSkip (dict{Part

list[tuple(x,y)]}): Set copies to skip. Here x and y are the indices in 2D space of copy , which needs to be skipped.

param seedOnly

If True, pattern the entities only along the first row and first column.

type seedOnly

bool

Returns: list[Part]: List of parts created.

createPipe(path, section='CIRCLE', size=0.01, width=0.01, thickness=0.0, angle=None, ignoredFeatures=None, propagate=False, resultType='COMBINE')

Create Pipe for FeatureCurve.

param path

type path

list[FeatureCurve]

param section

The Pipe profile type. Valid choices are: CIRCLE, SQUARE, TRIANGLE and RECTANGLE.

type section

str

param size

Length of the pipe. If value is a string it can be a Model Variable or a value with units.

type size

float | str

param width

Width of the pipe, only applicable for Rectangular profile.

type width

float

param thickness

Pipe thickness. If not set or set to zero, it will be solid pipe. If value is a string it can be a Model Variable or a value with units.

type thickness

float | str

param angle

Angle in radians. Only for xy alignment.

type angle

float

param ignoredFeatures

Ignored Features. Not mandatory. In propagated cases, if we need to ignore certain curves.

param propagate

if True enables propagate option, otherwise disabled.

type propagate

bool

param resultType

Valid values are: COMBINE, SUBTRACT, INTERSECT and NEW_PART.

type resultType

str

returns

New part created.

rtype

Part

moveFaces(features, position, duplicate=False)

Translate, rotate, copy, or extend features.

param features

The features to move.

type features

list[FeatureArea]

param position

The position to move the features at.

type position

math.Matrix44

param duplicate

If True, copy the features at given position.

type duplicate

bool

intersect(parts, createSolids=False, keepSourceParts=False)

Intersect tool that deletes excess faces, edges and vertices.

param parts

Parts to intersect.

type parts

list[Part]

param createSolids

If True, faces of solid volumes automatically selected.

type createSolids

bool

param keepSourceParts

Determines whether to keep source parts or not. When original parts are not kept, they are deleted from the model at the end of a successful operation.

type keepSourceParts

bool

returns

New part if created otherwise none.

rtype

Part/None

convertToMass(parts, parent=None)

Replace Parts to concentrated mass.

param parts

Parts to be replaced with concentrated mass.

type parts

list[Part]

param parent

Parent for the mass created.

type parent

Part

replaceFromFile(part, filePath)

Replace part with the contents of a file.

param part

The part to be replaced.

type part

Part

param filePath

The path to the file whose contents will replace the part.

type filePath

str

replaceFromPart(part, toolPart, keepToolPart=False)

Replace part with tool part.

param part

The part to be replaced.

type part

Part

param toolPart

The part to replace with.

type toolPart

Part

param keepToolPart

Determines whether to keep the toolPart or not after replace.

type keepToolPart

bool

circularPattern(input, axis, angle=60, count=3, equalSpacing=False, instances=False, symmetry=False, axisReverse=False, copiesToSkip=None)

Circular Pattern parts or faces around an axis.

param input

type input

list[Part] | list[FeatureArea]

param axis

Axis is a reference line, edge, or axis to which the pattern will be parallel.

type axis

math.Vector | FeatureCurve | System

param angle

Angle within which the copies are equally spaced.

type angle

float

param count

Number of copies.

type count

int

param equalSpacing

If True, equally space the copies within a specified Angle.

type equalSpacing

bool

param instances

If True, any changes to part or face will apply to all instances.

type instances

bool

param symmetry

Symmetry in Direction 1.

type symmetry

bool

param axisReverse

Reverse the axis in Direction 1.

type axisReverse

bool

param copiesToSkip (dict{Part

list[indicesToSkip]}): Set copies to skip. It’s basically a dictionary which contains Part as a key and list of indices to skip as values.

Returns: list[Part]: List of parts created.

draft(features, direction, neutralPlane, angle1=3.0, angle2=3.0, flipDrawDirection1=False, flipDrawDirection2=False)

Add draft to one or more faces of a part when designing a product that is manufactured using injection molding.

param features

Faces to Draft.

type features

list[FeatureArea]

param direction

The Draft direction. Valid values are: SINGLE, BOTH and SYMMETRY.

type direction

str

param neutralPlane

A reference plane or an existing face in the model. neutralPlane can not be same as draft feature.

type neutralPlane

FeaturePlanar, System

param angle1

The angle1 of draft.

type angle1

float

param angle2

The angle2 of draft. This is applicable for BOTH or SYMMETRY value for direction.

type angle2

float

param flipDrawDirection1

If True, flips the draw direction of draft in single direction.

type flipDrawDirection1

bool

param flipDrawDirection2

If True, flips the draw direction of draft. Applicable for BOTH direction.

type flipDrawDirection2

bool

convertBodiesToParts(parts)

Convert disconnected bodies to parts.

param parts

The parts to be converted.

type parts

list[Part]

returns

Newly created parts.

rtype

list[Part]

breakInstance(parts)

Break the instances of a part.

param parts

Parts for breaking instances.

type parts

list[Part]

projectAndSplit(targets, tools, direction, vectorDirection=None, extendProjection=True, extractProjection=False, surfaceNormal=None)

Project tools onto targets in a specified direction and splits the targets.

param targets

List of Parts or features on which feature projection to be.

type targets

list[Part] | list[Feature]

param tools

Feature that needs to be projected on Part.

type tools

list[Feature]

param direction

Valid values are: TOOL_NORMAL, X, Y, Z, VECTOR and CLOSEST_POINT, SURFACE_NORMAL.

type direction

str

param vectorDirection

Vector direction, only applicable when direction is ‘VECTOR’.

type vectorDirection

FeatureLinear | System

param extendProjection

If True, extends the projection.

type extendProjection

bool

param extractProjection

If True, extract projection without split.

type extractProjection

bool

param surfaceNormal

Planar surface along whose normal you want to project the tools.

type surfaceNormal

FeaturePlanar

Returns: list[Part]: List of parts created.

revolve2(profiles, axis, direction='SIGLE', resultType='NEW_PART', mergeTargets=None, flipAxis=False, angle1=0, angle2=0)

New Revolve - Revolve a face, sketch, line, or 2D edge about an axis.

param profiles

A face, line, or 2D edge.

type profiles

FeatureArea | FeatureCurve

param axis

An edge, line, cylindrical

type axis

FeatureLinear | FeatureCircular | System

param hole or a System. If it is of type System it has to have systemType Axis.

Selecting an edge on another part projects the axis of revolution to the planar face that will be rotated.

param direction

Valid values are: SINGLE, BOTH and SYMMETRY.

type direction

str

param resultType

Valid values are: COMBINE, SUBTRACT, INTERSECT and NEW_PART.

type resultType

str

param mergeTargets

Explict merge targets for Result Type.

type mergeTargets

list[Feature]

param flipAxis

If True, axis will be flipped.

type flipAxis

bool

param angle1

The angle of revolution.

type angle1

float

param angle2

The angle of revolution when direction is Both.

type angle2

float

returns

New part created if resultType is NEW_PART.

rtype

Part|None

edgeFillet(feature, radius='3 mm', continuity='TANGENT')

Creates fillet on a Linear feature.

param feature

feature that needs to fillet.

type feature

Feature

param radius

Radius of the fillet.

type radius

float | str

param continuity

Valid values are: TANGENT and CURVATURE.

type continuity

str

sweep(profiles, path, solidProfile=None, sweepAsSolid=True, profileOrientation=True, propagate=True, pathIgnoredFeatures=None, guideCurves=None, pathDirection='DIRECTION_1', twistType='NO_TWIST', twistAngle=0, twistTurns=0, twistAngleDir2=0, twistTurnsDir2=0, resultType='NEW_PART', mergeWithAllParts=True, mergeParts=None, twist1Reverse=False, twist2Reverse=False, guideScale='UNIFORM')

Sweep a profile along a path to create a solid or 3D surface.

param profiles

A face or a closed sketch.

type profiles

FeatureArea | FeatureCurve

param path

Path for the sweep.

type path

list[FeatureCurve]

param solidProfile

Sweep profile as solid. Only applicable for solid cylinder.

type solidProfile

Part

param sweepAsSolid

If true, sweep as solids otherwise sweep as surfaces.

type sweepAsSolid

bool

param profileOrientation

If true, sweep orientation will be normal to the path otherwise parallel.

type profileOrientation

bool

param propagate

If true, all the tangent edges of the input path is also selected.

type propagate

bool

param pathIgnoredFeatures

Edge to be ignored when propagate is True.

type pathIgnoredFeatures

list[FeatureCurve]

param guideCurves

Guide curves for the sweep. No guide curves are set by default.

type guideCurves

list[FeatureCurve]

param pathDirection

Sweep direction. - DIRECTION_1 - DIRECTION_2 - BOTH

type pathDirection

str

param twistType

Twist type. - NO_TWIST - ANGLE_TWIST - NO_OF_TURNS

type twistType

str

param twistAngle

Twist angle in DIRECTION_1.

type twistAngle

float

param twistTurns

Number of twist turns in DIRECTION_1.

type twistTurns

float

param twistAngleDir2

Twist angle in DIRECTION_2. Applicable only when pathDirection is “BOTH”.

type twistAngleDir2

float

param twistTurnsDir2

Number of twist turns in DIRECTION_2. Applicable only when pathDirection is “BOTH”.

type twistTurnsDir2

float

param resultType

Result type of sweep operation. - COMBINE - SUBTRACT - INTERSECT - NEW_PART

type resultType

str

param mergeWithAllParts

If True, merge with All parts otherwise merge with parts supplied in mergeTargets.

type mergeWithAllParts

bool

param mergeParts

Parts to be merged with sweep operation.

type mergeParts

Part

param twist1Reverse

If True, Reverse the twist in DIRECTION_1 or DIRECTION_2.

type twist1Reverse

bool

param twist2Reverse

If True, Reverse the twist in DIRECTION_2. Applicable only when pathDirection is “BOTH”.

type twist2Reverse

bool

param guideScale

Guide scale option. Applicable only when guideCurves is provided. - UNIFORM - LATERAL

type guideScale

str

returns

New part created if resultType is NEW_PART.

rtype

Part|None

nurbsCurve(controlPoints, nurbsCurveType='CURVE_OPEN', nurbsCurveDegree='DEGREE_3', controlPointWeight=None)

Create a NURBS curve, which is a free-form curve.

param controlPoints

List of control points to draw NURBS curve.

type controlPoints

list[FeaturePoints]

param nurbsCurveType

NURBS curve type. - CURVE_OPEN - CURVE_CLOSED - CURVE_PERIODIC - CURVE_NUM_TYPES

type nurbsCurveType

str

param nurbsCurveDegree

NURBS curve degree. - DEGREE_2 - DEGREE_3 - DEGREE_4 - DEGREE_5 - DEGREE_6 - DEGREE_7

type nurbsCurveDegree

str

param controlPointWeight

Index and weight for control point in NURBS curve.

type controlPointWeight

int, float

returns

New NURBS created.

rtype

Part

patternAlongPath(input, path, count=3, equalSpacing=False, spacing=0.01, instances=False, method='TRANSFORM', orientation='MAINTAIN_SEED_ORIENTATION', pathReverse=False, copiesToSkip=None)

Pattern parts or faces along curve.

Args: input (list[Part] | list[FeatureArea]): Parts or Features to create pattern

along the curve.

path (list[FeatureCurve]): Path for pattern. count (int): Number of copies. equalSpacing (bool): If True, equally space the copies. spacing (float): Distance between two copies. instances (bool): If True, any changes to part or face will apply to all instances. method (str): Pattern method.

• TRANSFORM

• OFFSET

orientation (str): Pattern Orientation.

• TANGENT_TO_CURVE

• MAINTAIN_SEED_ORIENTATION

pathReverse (bool): Reverse the path of pattern. copiesToSkip (dict{Part: list[indicesToSkip]}): Set copies to skip. It’s

basically a dictionary which contains Part as a key and list of indices to skip as values.

Returns: list[Part | Feature]: List of parts/features created.

multiSweep(profiles, path, sweepAsSolid=True, arcLengthProfiles=False, arcLengthGuides=False, orientation='PERPENDICULAR', normalToSurface=None, resultType='NEW_PART', mergeWithAllParts=True, mergeParts=None)

Sweep multiple profiles along a path to create a solid or surface.

param profiles

Faces or closed sketches.

type profiles

list[FeatureArea | FeatureCurve]

param path

Path for the multiSweep.

type path

list[FeatureCurve]

param sweepAsSolid

If true, sweep as solids otherwise sweep as surfaces.

type sweepAsSolid

bool

param arcLengthProfiles

If True, Set Arc Length Parametrization on profiles.

type arcLengthProfiles

bool

param arcLengthGuides

If True, Set Arc Length Parametrization on path.

type arcLengthGuides

bool

param orientation

Orientation for multiSweep. - PERPENDICULAR - PARALLEL - NORMAL_TO_SURFACE

type orientation

str

param normalToSurface

Face to which sweep orientation will be normal.

type normalToSurface

list[FeatureArea]

param resultType

Result type of multiSweep operation. - COMBINE - SUBTRACT - INTERSECT - NEW_PART

type resultType

str

param mergeWithAllParts

If True, merge with All parts otherwise merge with parts supplied in mergeTargets.

type mergeWithAllParts

bool

param mergeParts

Parts to be merged with sweep operation.

type mergeParts

Part

returns

New part created if resultType is NEW_PART.

rtype

Part|None

loft(profiles, loftAsSolid=True, guideCurves=None, arcLengthProfiles=False, arcLengthGuides=False, swapSurface=False, closed=False, resultType='NEW_PART', mergeWithAllParts=True, mergeParts=None)

Create a solid loft or a lofted surface from profiles and guide curves.

param profiles

Faces, closed sketches or curves.

type profiles

list[FeatureArea | FeatureCurve]

param loftAsSolid

If true, sweep as solids otherwise sweep as surfaces.

type loftAsSolid

bool

param guideCurves

Guide curves for the loft.

type guideCurves

list[FeatureCurve]

param arcLengthProfiles

If True, Set Arc Length Parametrization on profiles.

type arcLengthProfiles

bool

param arcLengthGuides

If True, Set Arc Length Parametrization on guides.

type arcLengthGuides

bool

param swapSurface

If True, interchange the profiles and rails to get preferred shape.

type swapSurface

bool

param closed

If True, close the loft.

type closed

bool

param resultType

Result type of loft operation. - COMBINE - SUBTRACT - INTERSECT - NEW_PART

type resultType

str

param mergeWithAllParts

If True, merge with All parts otherwise merge with parts supplied in mergeTargets.

type mergeWithAllParts

bool

param mergeParts

Parts to be merged with loft operation.

type mergeParts

Part

returns

New part created if resultType is NEW_PART.

rtype

Part|None

helixCurve(profile, type='TURNS_AND_HEIGHT', numTurns=2, pitch=0.003, height=0.01, startAngle=0, curveHand='RIGHT', heightReverse=False, lockDiameterRatio=True, topDiameter=0)

Create a solid loft or a lofted surface from profiles and guide curves.

param profile

Circular sketch profile.

type profile

FeatureCircular

param type

Helix Curve Type. - TURNS_AND_HEIGHT - TURNS_AND_PITCH - HEIGHT_AND_PITCH

type type

str

param numTurns

Number of turns in helix curve.

type numTurns

float

param pitch

Pitch distance of helix curve.

type pitch

float

param height

Height of helix curve.

type height

float

param startAngle

Start angle of helix curve.

type startAngle

float

param curveHand

Helix curve sweep direction. - LEFT - RIGHT

type curveHand

str

param heightReverse

If True, Reverse the height in other direction of helix curve.

type heightReverse

bool

param lockDiameterRatio

If True, Set lock diameter ratio of helix curve.

type lockDiameterRatio

bool

param topDiameter

Top Diameter of helix curve.

type topDiameter

float

returns

New part created.

rtype

Part

divideCurve(curve, divisionPoints, uniformDivision=False)

Divide a curve by inserting points along the curve.

param curve

Curve to divide.

type curve

FeatureCurve

param divisionPoints

List of divisionPoints (length ratio or length along the curve) and the bool value depicts position ratio. If True, Divide the curve on length ratio otherwise division occurs at length along the curve.

type divisionPoints

list(list[float], bool)

param uniformDivision

If True, Curve is uniformly divided.

type uniformDivision

bool

returns

New part created.

rtype

Part