SketchDimensions Object

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

Description

A collection of the dimensions in a sketch. This object also supports the methods to add new sketch dimensions.

Methods

Name	Description
addAngularDimension	Creates a new angular dimension constraint between the two input lines. The position of the text controls which of the four quadrants will be dimensioned.
addConcentricCircleDimension	Creates a new dimension constraint between to concentric circles or arcs.
addDiameterDimension	Creates a new diameter dimension constraint on the arc or circle.
addDistanceBetweenLineAndPlanarSurfaceDimension	Creates a new linear dimension controlling the distance between a sketch line and the specified planar face or construction plane. The sketch line must lie on a plane that is parallel to the planar surface. The text position is automatically chosen and is positioned so it is midway between the line and surface and the extension lines are a minimum length. You can modify the position by using functionality on the returned SketchDistanceBetweenLineAndPlanarSurfaceDimension object.
addDistanceBetweenPointAndSurfaceDimension	Creates a new linear dimension controlling the distance between a sketch point and the specified surface or point. The text position is automatically chosen and is positioned so it is midway between the point and surface and the extension lines are a minimum length. You can modify the position by using functionality on the returned SketchDistanceBetweenPointAndSurfaceDimension object.
addDistanceDimension	Creates a new linear dimension constraint between the two input entities.
addEllipseMajorRadiusDimension	Creates a new dimension constraint on the major radius of an ellipse.
addEllipseMinorRadiusDimension	Creates a new dimension constraint on the minor radius of an ellipse.
addLinearDiameterDimension	Creates a new linear dimension showing the diameter where the first line acts as the center line and the second entity defines the size. The first input entity must be a sketch line. The second entity can be a point or a line that is parallel to the first. The dimension controls the distance as measured perpendicular to the first input line.
addOffsetDimension	Creates a new linear dimension constraint between the two input entities. The first input entity must be a sketch line. The second entity can be a point or a line that is parallel to the first. The dimension controls the distance as measured perpendicular to the first input line.
addRadialDimension	Creates a new radial dimension constraint on the arc or circle.
addTangentDistanceDimension	Creates a new linear dimension from between a line and circle or arc and a second circle or arc where the dimension is to the tangent on the edge of the circle or arc.
classType	Static function that all classes support that returns the type of the class as a string. The returned string matches the string returned by the objectType property. For example if you have a reference to an object and you want to check if it's a SketchLine you can use myObject.objectType == fusion.SketchLine.classType().
item	Function that returns the specified sketch dimension using an index into the collection.

Properties

Name	Description
count	Returns the number of sketch dimensions in the sketch.
isValid	Indicates if this object is still valid, i.e. hasn't been deleted or some other action done to invalidate the reference.
objectType	This property is supported by all objects in the API and returns a string that contains the full name (namespace::objecttype) describing the type of the object. It's often useful to use this in combination with the classType method to see if an object is a certain type. For example: if obj.objectType == adsk.core.Point3D.classType():

Accessed From

Sketch.sketchDimensions

Samples

Name	Description
API Sample that demonstrates creating sketch lines in various ways.	Demonstrates several ways to create sketch lines, including as the result of creating a rectangle.
SketchDimensions.addAngularDimension	Demonstrates the SketchDimension.addAngularDimension method.
SketchDimensions.addConcentricCicleDimension	Demonstrates the SketchDimension.addConcentricCircleDimension method.
SketchDimensions.addDiameterDimension	Demonstrates the SketchDimension.addDiameterDimension method.
SketchDimensions.addDistanceDimension	Demonstrates the SketchDimension.addDistanceDimension method.
SketchDimensions.AddEllipseMajorRadiusDimension	Demonstrates the SketchDimension.addEllipseMajorRadiusDimension method.
SketchDimensions.AddEllipseMinorRadiusDimension	Demonstrates the SketchDimension.addEllipseMinorRadiusDimension method.
SketchDimensions.addOffsetDimension	Demonstrates the SketchDimension.addOffsetDimension method.

Version

Introduced in version August 2014