Sketch (hwx.common)#

class Sketch(Interface=None)#

Bases: object

Creates 2D parametric sketch geometry.

It is used to add items (points, lines, circles…) and constraints to them. Also contains sketch editing operations such as trim, fillet etc.

Attribute Table#

Name

Type

CONSTRAINT_ANGLE

int

CONSTRAINT_COINCIDENT

int

CONSTRAINT_COLLINEAR

int

CONSTRAINT_CONCENTRIC

int

CONSTRAINT_DIAMETER_ALIGNED

int

CONSTRAINT_DIAMETER_HORIZONTAL

int

CONSTRAINT_DIAMETER_VERTICAL

int

CONSTRAINT_DISTANCE_ALIGNED

int

CONSTRAINT_DISTANCE_HORIZONTAL

int

CONSTRAINT_DISTANCE_VERTICAL

int

CONSTRAINT_EQUAL

int

CONSTRAINT_FIXED

int

CONSTRAINT_HORIZONTAL

int

CONSTRAINT_HORIZONTAL_POINTS

int

CONSTRAINT_MAJOR_RADIUS

int

CONSTRAINT_MIDPOINT

int

CONSTRAINT_MINOR_RADIUS

int

CONSTRAINT_MIRROR

int

CONSTRAINT_OFFSET

int

CONSTRAINT_OFFSET_DISTANCE

int

CONSTRAINT_PARALLEL

int

CONSTRAINT_PERPENDICULAR

int

CONSTRAINT_RADIUS

int

CONSTRAINT_TANGENT

int

CONSTRAINT_VERTICAL

int

CONSTRAINT_VERTICAL_POINTS

int

DIMENSION_ANGLE

int

DIMENSION_DIAMETER_ALIGNED

int

DIMENSION_DIAMETER_HORIZONTAL

int

DIMENSION_DIAMETER_VERTICAL

int

DIMENSION_DISTANCE_ALIGNED

int

DIMENSION_DISTANCE_HORIZONTAL

int

DIMENSION_DISTANCE_VERTICAL

int

DIMENSION_MAJOR_RADIUS

int

DIMENSION_MINOR_RADIUS

int

DIMENSION_OFFSET_DISTANCE

int

DIMENSION_RADIUS

int

STATUS_FIXED

int

STATUS_FULLYDEFINED

int

STATUS_NOTCHANGED

int

STATUS_NOTCONSISTENT

int

STATUS_OVERDEFINED

int

STATUS_UNDERDEFINED

int

STATUS_UNKNOWN

int

TANGENT_INWARD

int

TANGENT_NORMAL_LEFT

int

TANGENT_NORMAL_RIGHT

int

TANGENT_OUTWARD

int

workplane

property
Method Table#

Name

Description

addArc3Points (self, start, end, third)

Adds an arc by defining three points.

addArcCenter2Points (self, center, point1, point2, ccw=True)

Adds an Arc defined by its center and its endpoints.

addArcTangentTo (self, tangentTo, start, end, bInvertTangent=False)

Adds an arc, starting tangent to a curve on a start point and ending on

addBoundedEllipse (self, center, majorAxisPoint, minorAxisPoint, start, end, bCounterClockWise=False)

Adds an ellipse defined by center, two points that define an axis and

addCircle2Points (self, point1, point2)

Adds a circle defined by the 2 endpoints of a diameter.

addCircle3Points (self, point1, point2, point3)

Adds a circle defined by three points.

addCircleCenterPoint (self, center, point)

Adds a circle defined by its center and one point.

addCircleCenterRadius (self, center, radius)

Adds a circle defined by its center and radius.

addConstraint (self, constraint, item1=None, item2=None, mirrorAxis=None)

Adds a constraint for one or two items.

addDimension (self, dimension, value=None, item1=None, item2=None, x=1.7976931348623157e+308, y=1.7976931348623157e+308, pickX=1.7976931348623157e+308, pickY=1.7976931348623157e+308)

Defines constrain the dimensions of a sketch.

addEllipse (self, center, verticalAxis, majorRadius, minorRadius=None)

Adds an ellipse defined by center, vertical axis and radius, or

addLine (self, point, direction)

Adds a line with the specified direction, that goes through a point.

addLineSegment (self, point1, point2)

Adds a line segment defined by two endpoints.

addParallelogram (self, lowerLeft, lowerRight, upperRight)

Adds a parallelogram defined 3 vertex.

addPoint (self, x, y)

addPolyline (self, points)

Adds a Polyline of line segments that go through the specified points.

addRectangle2Vertex (self, vertex1, vertex2)

Adds a rectangle aligned with sketch axis defined by two vertex.

addRectangle3Vertex (self, lowerLeft, lowerRight, upperRight)

Adds a rectangle defined by three vertex.

addRectangleCenter2Points (self, center, lengthPoint, widthPoint)

Adds a rectangle defined by center and two vertex.

addRectangleCenterVertex (self, center, vertex)

Adds a rectangle aligned with sketch axis defined by center and one vertex.

addRegularPolygon (self, center, point, numSides, beMidPoint=False)

Adds a regular polygon defined by center, one vertex and the number of sides.

addSpline (self, points, degree=3, periodic=False, interpolated=False)

Adds a spline based on a list of points.

circularPattern (self, entities, point, copy, angle, symmetry, createDimension=True, equalSpacing=False)

Pattern sketch entities around a point.

deleteItem (self, item)

Removes an item from the sketch.

enableHistory (self, state=True)

Set the state of the abilty to store history

evaluate (self)

Recalculates sketch items according to constraints.

extend (self, curvePoint, limitPoint)

Extend or shorten an entity of a sketch curve.

fillet (self, vertices, radius=0)

Fillet a list of vertices with the specified radius.

findCircle (self, uid)

Returns the Circle with the specified id.

findConstraint (self, uid)

Returns the Constraint with the specified id.

findEllipse (self, uid)

Returns the Ellipse with the specified id.

findItem (self, uid)

Returns the InterfaceItem with the specified id.

findLine (self, uid)

Returns the Line with the specified id.

findPoint (self, uid)

Returns the Point with the specified id.

findSpline (self, uid)

Returns the Spline with the specified id.

getActive ()

Sketch currently being edited in the gui.

getDimensionVariableName (self, dimension)

Gets the variable of a dimension.

getEndPoints (self, item)

Returns the item endpoints as a PointVector.

getItemStatus (self, item)

Returns the status of item according the ITEM_STATUS enum.

hasCircle (self, uid)

Returns True if sketch contains a Point with the specified id, False otherwise.

hasConstraint (self, uid)

Returns True if sketch contains a Point with the specified id, False otherwise.

hasEllipse (self, uid)

Returns True if sketch contains a Point with the specified id.

hasItem (self, uid)

Returns True if sketch contains a Point with the specified id, False otherwise.

hasLine (self, uid)

Returns True if sketch contains a Point with the specified id, False otherwise.

hasPoint (self, uid)

Returns True if sketch contains a Point with the specified id, False otherwise.

hasSpline (self, uid)

Returns True if sketch contains a Point with the specified id, False otherwise.

isAnyOverConstrained (self)

Returns True if and items are over constrained, False otherwise.

isConstruction (self, item)

Returns True if the item is a construction item, False otherwise.

isDimensionDriven (self, item)

Returns True if the item is a dimension and is driven, False otherwise.

isFixed (self, item)

Returns True if the item is fixed, False otherwise.

linearPattern (self, entities, direction1, copy1=3, distance1=0.1, symmetry1=False, direction2=None, copy2=3, distance2=0.1, symmetry2=False)

Pattern sketch entities in a linear direction.

mirror (self, curves, mirrorLine)

Creates symmetric copies of selected sketch curves across a selected

offset (self, point, distance)

Creates a copy of a sketch curve at a specified distance from the source curve.

origin (self)

Returns the Point for the origin.

parameterManager (self)

Return the Parameter Manager for this sketch

polylineAddArcTo (self, polyline, arcTo, direction)

Adds an arc from the polyline last point to the specified Point.

polylineAddLineTo (self, polyline, pointTo)

Adds a line segment from the polyline last point to the specified Point.

polylineEnd (self, polyline)

Finishs the construction of the polyline.

polylineStart (self, x, y)

Starts the creation of a polyline on a specified Point.

populate (self)

Redraws the sketch if required.

rotate (self, entities, center, angle, keepRelations=True)

Rotate Sketch entities.

setConstruction (self, item, state=True)

Set the items construction flag.

setDimensionIsDriven (self, item, state)

Returns True if the item is a dimension and is driven, False otherwise.

setDimensionVariable (self, dimension, varName)

Sets a variable as value for a dimension.

setFixed (self, item, state=True)

Set the items fixed state.

setParameterManager (self, pm)

Set the Parameter Manager to use for this sketch

setWorkplane (self, matrix)

Define the workplane from the passed matrix.

split (self, curvePoint, breakPoint)

Split a curve in two at a defined break point.

translate (self, entities, direction, value, keepRelations=True)

Translate Sketch entities.

trim (self, x, y)

Removes one or more geometric entities below the (x, y) coordinates of

update (self)

Evaluates and populates the sketch.

Example

Define and use Splines.#
from hwx import inspire
from hwx.common.Sketch import Sketch

model = inspire.newModel()

# instanciate sketch
s = Sketch()

# instantiate points
p1 = s.addPoint(2, 2)
p2 = s.addPoint(1, 1)

# we can also query and set the position of point p1.
position = p1.position
print(f'Position of p1: {position}')
p1.position = (0, 0)
print(f'Position of p1 after change: {p1.position}')

# instantiate line segment using points or coordinates
ls1 = s.addLineSegment(p1, p2)
ls2 = s.addLineSegment((2, 2), (4, 4))

# instantiate line using point and direction
l1 = s.addLine((3, 3), (1, -1))
# we can also query the position of line l1.
print(f'Position and direction of l1 : {l1.position}, {l1.direction}')
s.addLine(p1, (1, 0))
setWorkplane(matrix)#

Define the workplane from the passed matrix.

isConstruction(item)#

Returns True if the item is a construction item, False otherwise.

setConstruction(item, state=True)#

Set the items construction flag.

isFixed(item)#

Returns True if the item is fixed, False otherwise.

setFixed(item, state=True)#

Set the items fixed state.

isAnyOverConstrained()#

Returns True if and items are over constrained, False otherwise.

enableHistory(state=True)#

Set the state of the abilty to store history

addPoint(x, y)#

Adds a Point to the Sketch at defined position.

Parameters:

  • x (float) – The x coordinate of the point.

  • y (float) – The y coordinate of the point.

Returns:

The new Point.

Return type:

Point

addLine(point, direction)#

Adds a line with the specified direction, that goes through a point.

Parameters:

  • point (Point | tuple[float, float]) – The point of the line.

  • direction (tuple[float, float]) – The direction of the line.

Returns:

The new line.

Return type:

Line

addLineSegment(point1, point2)#

Adds a line segment defined by two endpoints.

Parameters:

  • point1 (Point | tuple[float, float]) – The endpoint of the line.

  • point2 (Point | tuple[float, float]) – The endpoint of the line.

Returns:

The new line segment.

Return type:

Line

addCircleCenterRadius(center, radius)#

Adds a circle defined by its center and radius.

Parameters:

  • center (Point | tuple[float, float]) – The center of the circle.

  • radius (float) – The radius of the circle.

Returns:

The new circle.

Return type:

Circle

addCircleCenterPoint(center, point)#

Adds a circle defined by its center and one point.

Parameters:

  • center (Point | tuple[float, float]) – The center of the circle.

  • point (Point | tuple[float, float]) – The point of the circle.

Returns:

The new circle.

Return type:

Circle

addCircle2Points(point1, point2)#

Adds a circle defined by the 2 endpoints of a diameter.

Parameters:

  • point1 (Point | tuple[float, float]) – The endpoint of the diameter.

  • point2 (Point | tuple[float, float]) – The endpoint of the diameter.

Returns:

The new circle.

Return type:

Circle

addCircle3Points(point1, point2, point3)#

Adds a circle defined by three points.

Parameters:

  • point1 (Point | tuple[float, float]) – The point of the circle.

  • point2 (Point | tuple[float, float]) – The point of the circle.

  • point3 (Point | tuple[float, float]) – The point of the circle.

Returns:

The new circle.

Return type:

Circle

addArcCenter2Points(center, point1, point2, ccw=True)#

Adds an Arc defined by its center and its endpoints.

Parameters:

  • center (Point | tuple[float, float]) – The center of the arc.

  • point1 (Point | tuple[float, float]) – The point of the circle.

  • point2 (Point | tuple[float, float]) – The point of the circle.

  • ccw (bool) – Determines whether to use counter clockwise direction from point1 to point2 or not.

Returns:

The new arc.

Return type:

Circle

addArc3Points(start, end, third)#

Adds an arc by defining three points.

Parameters:

  • start (Point | tuple[float, float]) – The start point of the arc.

  • end (Point | tuple[float, float]) – The end point of the arc.

  • third (Point | tuple[float, float]) – An another point of the arc.

Returns:

The new arc.

Return type:

Circle

addArcTangentTo(tangentTo, start, end, bInvertTangent=False)#
Adds an arc, starting tangent to a curve on a start point and ending on

a defined point.

Parameters:

  • tangentTo (InterfaceItem) – The item to be tangent to.

  • start (Point | tuple[float, float]) – The point where the arc starts.

  • end (Point | tuple[float, float]) – The end point of the arc.

  • bInvertTangent (bool) – Determines whether to construct the arc with inverted tangent.

Returns:

The new arc.

Return type:

Circle

addEllipse(center, verticalAxis, majorRadius, minorRadius=None)#
Adds an ellipse defined by center, vertical axis and radius, or

by center Point, and Line for major axis and Line for minor axis.

Parameters:

  • center (Point | tuple[float, float]) – The center of the ellipse.

  • verticalAxis (Line | tuple[float, float]) – For a Line, the majorAxis, otherwise the vertical axis of the ellipse.

  • majorRadius (Line | float) – For a Line, the minor axis, otherwie the major radius of the ellipse.

  • minorRadius (float) – The minor radius of the ellipse.

Returns:

The new ellipse.

Return type:

Ellipse

addBoundedEllipse(center, majorAxisPoint, minorAxisPoint, start, end, bCounterClockWise=False)#

Adds an ellipse defined by center, two points that define an axis and start and end points.

Parameters:

  • center (Point | tuple[float, float]) – The center of the ellipse.

  • majorAxisPoint (Line | tuple[float, float]) – The start point defining the major axis.

  • minorAxisPoint (Line | tuple[float, float]) – The end point defining the major axis.

  • start (Point | tuple[float, float]) – The start point of the ellipse.

  • end (Point | tuple[float, float]) – The end point of the ellipse.

  • bCounterClockWise (bool) – Determines whether to use counter clockwise direction from start to end or not.

Returns:

The new ellipse.

Return type:

Ellipse

addSpline(points, degree=3, periodic=False, interpolated=False)#

Adds a spline based on a list of points.

Parameters:

  • points (list[tuple[float, float]]| list[Point]) – The points of the spline.

  • degree (int) – The degree.

  • periodic (bool) – Determines whether it is periodic.

  • interpolated (bool) – Determines whether it should get interpolated.

Returns:

The new spline.

Return type:

Spline

addPolyline(points)#

Adds a Polyline of line segments that go through the specified points.

Parameters:

  • (list[tuple[float (points) – The points of the polyline.

  • float]] – The points of the polyline.

Returns:

The new created polyline.

Return type:

Polyline

polylineStart(x, y)#

Starts the creation of a polyline on a specified Point.

Parameters:

  • x (float) – The x coordinate of the first point.

  • y (float) – The y coordinate of the first point.

Returns:

The new created polyline.

Return type:

Polyline

polylineAddLineTo(polyline, pointTo)#

Adds a line segment from the polyline last point to the specified Point.

Parameters:

  • polyline (Polyline) – The polyline that is being constructed.

  • pointTo (tuple[float, float]) – The position of the endpoint of the new line.

Returns:

True if the arc was successfully added to the polyline, False otherwise.

Return type:

bool

polylineAddArcTo(polyline, arcTo, direction)#

Adds an arc from the polyline last point to the specified Point.

Parameters:

  • polyline (Polyline) – The polyline that is being constructed.

  • arcTo (tuple[float, float]) – The position of the endpoint of the new arc.

  • direction (enum) – The initial direction of the arc.

Returns:

True if the arc was successfully added to the polyline, False otherwise.

Return type:

bool

polylineEnd(polyline)#

Finishs the construction of the polyline.

Parameters:

polyline (Polyline) – The polyline that is being constructed.

Returns:

The points and lines of the polyline.

Return type:

tuple[list[Points], list[Lines]]

addRectangleCenterVertex(center, vertex)#

Adds a rectangle aligned with sketch axis defined by center and one vertex.

Parameters:

  • center (tuple[float, float]) – The center of the rectangle.

  • vertex (tuple[float, float]) – A vertex of the rectangle.

Returns:

The points and lines of the rectangle.

Return type:

tuple[list[Points], list[Lines]]

addRectangle2Vertex(vertex1, vertex2)#

Adds a rectangle aligned with sketch axis defined by two vertex.

Parameters:

  • vertex1 (tuple[float, float]) – A vertex of the rectangle.

  • vertex2 (tuple[float, float]) – A vertex of the rectangle.

Returns:

The points and lines of the rectangle.

Return type:

tuple[list[Points], list[Lines]]

addRectangle3Vertex(lowerLeft, lowerRight, upperRight)#

Adds a rectangle defined by three vertex.

Parameters:

  • lowerLeft (tuple[float, float]) – The lower left point of the rectangle.

  • lowerRight (tuple[float, float]) – The lower right point of the rectangle.

  • upperRight (tuple[float, float]) – The upper right point of the rectangle.

Returns:

The points and lines of the rectangle.

Return type:

tuple[list[Points], list[Lines]]

addRectangleCenter2Points(center, lengthPoint, widthPoint)#

Adds a rectangle defined by center and two vertex.

Parameters:

  • center (tuple[float, float]) – The center of the rectangle.

  • lengthPoint (tuple[float, float]) – A vertex of the rectangle.

  • widthPoint (tuple[float, float]) – A vertex of the rectangle.

Returns:

The points and lines of the rectangle.

Return type:

tuple[list[Points], list[Lines]]

addParallelogram(lowerLeft, lowerRight, upperRight)#

Adds a parallelogram defined 3 vertex.

Parameters:

  • lowerLeft (tuple[float, float]) – The lower left point of of the parallelogram.

  • lowerRight (tuple[float, float]) – The lower right point of of the parallelogram.

  • upperRight (tuple[float, float]) – The lower right point of of the parallelogram.

Returns:

The points and lines of the parallelogram.

Return type:

tuple[list[Points], list[Lines]]

addRegularPolygon(center, point, numSides, beMidPoint=False)#

Adds a regular polygon defined by center, one vertex and the number of sides.

Parameters:

  • center (tuple[float, float]) – The center of the regular polygon.

  • point (tuple[float, float]) – A vertex of the regular polygon.

  • numSides (int) – The number of sides.

  • beMidPoint (bool) –

Returns:

The points and lines of the rectangle.

Return type:

tuple[list[Points], list[Lines]]

addConstraint(constraint, item1=None, item2=None, mirrorAxis=None)#

Adds a constraint for one or two items.

Parameters:

  • constraint (enum) – The constraint.

  • item1 (InterfaceItem) – The item to hold the constraint.

  • item2 (InterfaceItem) – The item to hold the constraint.

  • mirrorAxis (InterfaceItem) – The item for a mirror constraints axis.

Returns:

The new constraint.

Return type:

Constraint

addDimension(dimension, value=None, item1=None, item2=None, x=1.7976931348623157e+308, y=1.7976931348623157e+308, pickX=1.7976931348623157e+308, pickY=1.7976931348623157e+308)#

Defines constrain the dimensions of a sketch.

Parameters:

  • dimension (enum) – The type of dimension.

  • value – The value of the dimension.

  • item1 (InterfaceItem) – The item to hold the constraint.

  • item2 (InterfaceItem) – The item to hold the constraint.

Returns:

The new dimension.

Return type:

Dimension

isDimensionDriven(item)#

Returns True if the item is a dimension and is driven, False otherwise.

setDimensionIsDriven(item, state)#

Returns True if the item is a dimension and is driven, False otherwise.

deleteItem(item)#

Removes an item from the sketch.

Parameters:

item (InterfaceItem) – The item to be removed.

Returns:

True if the item has been successfully removed, False otherwise.

Return type:

bool

getEndPoints(item)#

Returns the item endpoints as a PointVector.

getItemStatus(item)#

Returns the status of item according the ITEM_STATUS enum.

setDimensionVariable(dimension, varName)#

Sets a variable as value for a dimension.

Parameters:

  • dimension (Constraint) – The dimension.

  • varName (str) – The name of the variable.

getDimensionVariableName(dimension)#

Gets the variable of a dimension.

Parameters:

dimension (Constraint) – The dimension.

Returns:

The name of the variable.

Return type:

str

update()#

Evaluates and populates the sketch.

populate()#

Redraws the sketch if required.

evaluate()#

Recalculates sketch items according to constraints.

origin()#

Returns the Point for the origin.

findPoint(uid)#

Returns the Point with the specified id.

findLine(uid)#

Returns the Line with the specified id.

findCircle(uid)#

Returns the Circle with the specified id.

findEllipse(uid)#

Returns the Ellipse with the specified id.

findSpline(uid)#

Returns the Spline with the specified id.

findConstraint(uid)#

Returns the Constraint with the specified id.

findItem(uid)#

Returns the InterfaceItem with the specified id.

hasPoint(uid)#

Returns True if sketch contains a Point with the specified id, False otherwise.

hasLine(uid)#

Returns True if sketch contains a Point with the specified id, False otherwise.

hasCircle(uid)#

Returns True if sketch contains a Point with the specified id, False otherwise.

hasEllipse(uid)#

Returns True if sketch contains a Point with the specified id.

hasSpline(uid)#

Returns True if sketch contains a Point with the specified id, False otherwise.

hasConstraint(uid)#

Returns True if sketch contains a Point with the specified id, False otherwise.

hasItem(uid)#

Returns True if sketch contains a Point with the specified id, False otherwise.

split(curvePoint, breakPoint)#

Split a curve in two at a defined break point.

Parameters:

  • curvePoint (tuple[float, float]) – The point of the curve to be splitted.

  • breakPoint (tuple[float, float]) – The point of break.

Returns:

True on success, False otherwise.

Return type:

bool

extend(curvePoint, limitPoint)#

Extend or shorten an entity of a sketch curve.

Parameters:

  • curvePoint (tuple[float, float]) – The point of the curve to extend.

  • limitPoint (tuple[float, float]) – The point of the limit curve.

Returns:

True on success, False otherwise.

Return type:

bool

fillet(vertices, radius=0)#

Fillet a list of vertices with the specified radius.

Parameters:

  • vertices (list[Points],) – The vertices to be filleted.

  • radius (float) – The fillet radius.

Returns:

True on success, False otherwise.

Return type:

bool

mirror(curves, mirrorLine)#

Creates symmetric copies of selected sketch curves across a selected centerline.

By default, there is a parent-child relationship between source curves and their symmetric copies.

Parameters:

  • vertices (list[InterfaceItem]) – The curves to be mirrored.

  • mirrorLine (Line) – The mirror line.

Returns:

True if all items have been mirrored, False otherwise.

Return type:

bool

trim(x, y)#

Removes one or more geometric entities below the (x, y) coordinates of the sketch curve.

Parameters:

  • x (float) – The x coordinate.

  • y (float) – The y coordinate.

Returns:

True if a geometric entity was trimmed, False otherwise.

Return type:

bool

offset(point, distance)#

Creates a copy of a sketch curve at a specified distance from the source curve.

Parameters:

  • point (tuple[float, float]) –

  • distance (float) –

Returns:

True on success, False otherwise.

Return type:

bool

linearPattern(entities, direction1, copy1=3, distance1=0.1, symmetry1=False, direction2=None, copy2=3, distance2=0.1, symmetry2=False)#

Pattern sketch entities in a linear direction.

Parameters:

  • entities (list[SketchItem]) – Sketch curve entity to create linear pattern.

  • direction1 (Line) – Direction 1 for sketch pattern.

  • copy1 (int) – Number of copies in direction 1.

  • distance1 (float) – Distance between two copies in direction 1.

  • symmetry1 (bool) – Symmetry in Direction 1.

  • direction2 (Line) – Direction 2 for sketch pattern.

  • copy2 (int) – Number of copies in direction 2.

  • distance2 (float) – Distance between two copies in direction 2.

  • symmetry2 (bool) – Symmetry in Direction 2.

Returns:

LinearPattern Object.

Return type:

LinearPattern

circularPattern(entities, point, copy, angle, symmetry, createDimension=True, equalSpacing=False)#

Pattern sketch entities around a point.

Parameters:

  • entities (list[SketchItem]) – Sketch curve entity to create linear pattern.

  • point (Point) – Center Point for circular sketch pattern.

  • copy (int) – Number of copies.

  • angle (float) – Distance between two copies in direction 1.

  • symmetry (bool) – Symmetry in Direction 1.

  • createDimension (bool) – If True, dimension is added otherwise not.

  • equalSpacing (bool) – If True, equally space the copies otherwise not.

Returns:

CircularPattern Object.

Return type:

CircularPattern

translate(entities, direction, value, keepRelations=True)#

Translate Sketch entities.

Parameters:

  • entities (list[SketchItem]) – Sketch entity to translate.

  • direction (tuple[float, float]) – Direction for sketch translation.

  • value (float) – Translate value for sketch entity.

  • keepRelations (bool) – Keep relations between sketch entities after translation.

Returns:

True on success, False otherwise.

Return type:

bool

rotate(entities, center, angle, keepRelations=True)#

Rotate Sketch entities.

Parameters:

  • entities (list[SketchItem]) – Sketch entity to rotate.

  • center (Point) – Center point to rotate sketch entity.

  • angle (float) – Rotation angle for sketch entity.

  • keepRelations (bool) – Keep relations between sketch entities after rotation.

Returns:

True on success, False otherwise.

Return type:

bool

parameterManager()#

Return the Parameter Manager for this sketch

setParameterManager(pm)#

Set the Parameter Manager to use for this sketch