Sketch.addCenterPointArcSlot Method

Parent Object: Sketch
Defined in namespace "adsk::fusion" and the header file is <Fusion/Sketch/Sketch.h>

Description

Creates the geometry that represents a center-point arc slot. The center point defines the center of the slot and the end point defines the center of the end of the slot. The width of the slot is defined by a value and optionally the radius and angle can be specified. Geometric constraints are automatically added to the geometry to maintain the slot shape, and optionally, dimensions are created to control the size. The created geometry and dimensions are returned.

Syntax

"sketch_var" is a variable referencing a Sketch object.

# Uses no optional arguments.
returnValue = sketch_var.addCenterPointArcSlot(centerPoint, startPoint, endPoint, width)

# Uses optional arguments.
returnValue = sketch_var.addCenterPointArcSlot(centerPoint, startPoint, endPoint, width, radius, angle, createWidthDimension, createRadiusDimension, createAngleDimension)
"sketch_var" is a variable referencing a Sketch object.

#include <Fusion/Sketch/Sketch.h>

// Uses no optional arguments.
returnValue = sketch_var->addCenterPointArcSlot(centerPoint, startPoint, endPoint, width);

// Uses optional arguments.
returnValue = sketch_var->addCenterPointArcSlot(centerPoint, startPoint, endPoint, width, radius, angle, createWidthDimension, createRadiusDimension, createAngleDimension);
"sketch_var" is a variable referencing a Sketch object.

// Uses no optional arguments.
returnValue = sketch_var.addCenterPointArcSlot(centerPoint, startPoint, endPoint, width);

// Uses Optional arguments.
returnValue = sketch_var.addCenterPointArcSlot(centerPoint, startPoint, endPoint, width, radius, angle, createWidthDimension, createRadiusDimension, createAngleDimension);

Return Value

Type Description
Base[] Returns an array containing the start point arc, the end point arc, the two arcs that define the sides of the slot, the construction arc that runs through the center of the slot, and optionally the width, radius, and angle dimension constraints that were created. If an angle constraint was created, the array also includes the two supporting construction lines used by the angular dimension: a radius construction line from the slot center to the start of the slot's center arc, followed by the horizontal construction line that was created (and that has a horizontal geometric constraint applied). Returns an empty array if the operation failed.

Parameters

Name Type Description
centerPoint Base The center point of the center arc of the slot. It can be a SketchPoint or Point3D object. If a SketchPoint is provided, the slot becomes dependent on that point and will recompute if the point moves.
startPoint Base The start point of the center arc of the slot. It can be a SketchPoint or Point3D object. The distance from the centerPoint to this point defines the radius of the slot's center arc unless the radius argument is supplied, in which case the radius argument defines the radius, and this point is used only for its direction from the centerPoint. If a SketchPoint is provided, the slot becomes dependent on that point and will recompute if the point moves.
endPoint Base A point that defines the center of the end of the slot. It can be a SketchPoint or Point3D object. If values are specified for the radius or angle, this point no longer defines the exact center of the end but is used to define the direction or quadrant the end point is in.
width ValueInput A ValueInput object that defines the width of the slot. The ValueInput can define either a real value or an expression string. If it is a real value, it defines the width of the slot in centimeters.

When using a ValueInput created using a string, it's the same as creating a parameter in the user-interface. You can specify any valid expression, i.e. "5", "5 in", "5 in / 2", "5 + Length" that defines a length.

The width must be greater than zero and strictly less than twice the radius of the base arc, otherwise the slot is invalid.
radius ValueInput An optional ValueInput object that defines the radius of the slot from the center to the end point (i.e. the radius of the slot's center arc). The ValueInput can define either a real value or an expression string. If it is a real value, it specifies the slot radius in centimeters.

The radius must be greater than zero otherwise the slot is invalid.

This is an optional argument whose default value is null.
angle ValueInput An optional ValueInput object that defines the angle of the slot as measured from a horizontal line. The ValueInput can define either a real value or an expression string. If it is a real value, it defines the angle of the slot in radians; if it's an expression it must define an angle.

This is an optional argument whose default value is null.
createWidthDimension boolean Specifies if a dimension constraint and its associated parameter is created to control the width of the slot.

This is an optional argument whose default value is False.
createRadiusDimension boolean Specifies if a dimension constraint and its associated parameter is created to control the radius of the slot.

This is an optional argument whose default value is False.
createAngleDimension boolean Specifies if a dimension constraint and its associated parameter is created to control the angle of the slot. If this is true, a horizontal line is also created for the dimension to go between it and the center arc of the slot.

This is an optional argument whose default value is False.

Version

Introduced in version September 2026