Sketcher

sketcherAPI

Provides functions for interaction with the classcad sketcher api.

addConstraints

Adds constraint to sketch

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, names: string[], cctypes: string[], entitiesArray: ObjectID[][], userValues?: (number | string)[], dimPoses?: PointMemValue[], dimInitialisationOptions?: any[]): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch
names	string[]		New constraint name
cctypes	string[]		New constraint class
entitiesArray	ObjectID[][]		Involved geometry objects
userValues?	(number l string)[]		Only for angle constraint
dimPoses?	PointMemValue[]		For CreateDimension
dimInitialisationOptions?	any[]		For CreateDimension

Returns Promise<void>

addGeometry

Adds geometry object to sketch

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, type: 'Point' | 'Line' | 'Arc' | 'Circle', params: PointType | LineType | ArcType | CircleType, autoConstr: autoConstrT, restrictions?: RestrictionType[], restrictionValues?: any[], startPointRestrictions?: RestrictionType[], startPointRestrictionValues?: any[]): Promise<ObjectID | null>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch
type	'Point' l 'Line' l 'Arc' l 'Circle'		Type of object to add - "Point", "Line", "Arc", "Circle"
params	PointType l LineType l ArcType l CircleType		Parameter for a point, line, arc or circle depending on type parameter
autoConstr	autoConstrT
restrictions?	RestrictionType[]		(optional) - array of restriction tokens
restrictionValues?	any[]		(optional) - array of restriction values
startPointRestrictions?	RestrictionType[]		(optional) - array of restriction tokens for the start point
startPointRestrictionValues?	any[]		(optional) - array of restriction values for the start point

Returns Promise<ObjectID | null>
The id of the new created geometry or null.

addPolycurveSegment

Adds a line or a curve with spicified parameters and creates an incidence constraint between its start point and another point

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, incidentPointId: ObjectID, params: LineType | ArcType, autoConstr: autoConstrT, restrictions?: RestrictionType[], restrictionValues?: number[], startPointRestrictions?: RestrictionType[], startPointRestrictionValues?: number[]): Promise<ObjectID | null>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch
incidentPointId	ObjectID		Id of another point for incidence constraint
params	LineType l ArcType		Array of parameters for a curve or line
autoConstr	autoConstrT
restrictions?	RestrictionType[]		(optional) - array of restriction tokens
restrictionValues?	number[]		(optional) - array of restriction values
startPointRestrictions?	RestrictionType[]		(optional) - array of restriction tokens for the start point
startPointRestrictionValues?	number[]		(optional) - array of restriction values for the start point

Returns Promise<ObjectID | null>
The id of the new created object or null.

addSketchRegion

Adds a new sketch region

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, name: string, curves: ObjectID[]): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch
name	string		Name of the new sketch region
curves	ObjectID[]		Array of curve ids to represent the sketch region

Returns Promise<void>

changeReferenceGeometry

Re-links "Use"-Geometry in sketch - the same geometry will be connected to another referene

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, useGeometryId: ObjectID, referenceId: ObjectID): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch which the geometry belongs to
useGeometryId	ObjectID		Id of the CC_Arc/Circle/Line/Point that should be re-linked
referenceId	ObjectID		Id of the new edge / vertex to be referenced

Returns Promise<void>

closePolyLine

Creates a line between 2 points and incidence constraints between its start / end points and corresponding points

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, startPointId: ObjectID, endPointId: ObjectID): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch
startPointId	ObjectID		Id of the start point
endPointId	ObjectID		Id of the end point

Returns Promise<void>

copyCircularPattern

Copies selected rigidset (or singular object) in circular pattern

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, rigidsetId: ObjectID, rotationOrigin: PointMemValue, angleStep: number, count: number): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch containing selected rigidset
rigidsetId	ObjectID		Id of selected rigidset
rotationOrigin	PointMemValue		Point to be used as an origin for rotation
angleStep	number		Angular offset between neighbouring copied objects
count	number		Number of copies

Returns Promise<void>

copyMirrorPattern

Copies selected rigidset (or singular object) in mirror pattern

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, rigidsetId: ObjectID, symmetricLineId: ObjectID): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch containing selected rigidset
rigidsetId	ObjectID		Id of selected rigidset
symmetricLineId	ObjectID		Id of the line to be used as a symmetric line

Returns Promise<void>

copyObjects

Copies selected objects of the sketch

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, objectIds: ObjectID[], translate: number, toCopyConstraints: boolean): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch containing selected objects
objectIds	ObjectID[]		An array of selected object ids
translate	number		Offset from initial objects
toCopyConstraints	boolean		A flag allowing to restrict copying constraints from original selected objects

Returns Promise<void>

copyRectangularPattern

Copies selected rigidset (or singular object) in rectangular pattern

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, rigidsetId: ObjectID, originIndex: {

index: number;

memberName?: string;

}, translate: PointMemValue, xCount: number, yCount: number): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch containing selected rigidset
rigidsetId	ObjectID		Id of selected rigidset
originIndex.index	number
originIndex.memberName?	string
translate	PointMemValue		Vector with horizontal / vertical offset between neighbouring copied objects
xCount	number		Number of copies along the x-axis
yCount	number		Number of copies along the y-axis

Returns Promise<void>

copySketch

Copies the sketch elements from one sketch to another

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, toCopySketchId: ObjectID): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the existing sketch to copy sketch elements into it
toCopySketchId	ObjectID		Id of the sketch to copy elements from

Returns Promise<void>

createAndSetWorkPlane

Creates and sets workplane from the selected face for the sketcher

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, faceId: ObjectID): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch
faceId	ObjectID		Id of the face

Returns Promise<void>

createFillet

Creates a fillet in place of a point connecting 2 lines

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, lineIds: ObjectID[], lineStartIds: ObjectID[], incidenceId: ObjectID, control: PointMemValue, start: PointMemValue, mid: PointMemValue, end: PointMemValue): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch
lineIds	ObjectID[]		Array of 2 line ids
lineStartIds	ObjectID[]		Array of ids of 2 points of different lines which are incident to the selected point
incidenceId	ObjectID		Id of the incidence constraint which connects lineStart points
control	PointMemValue		Position of the selected point
start	PointMemValue		Position of the beginning of an arc
mid	PointMemValue		Position of the middle of an arc
end	PointMemValue		Position of the ending of an arc

Returns Promise<void>

createRectangle

Creates a rectangle formed with 2 points

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, start: PointMemValue, end: PointMemValue, options?: RectOptionsType): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		ObjectID - id of the sketch
start	PointMemValue		The 1st point to form rectangle
end	PointMemValue		The 2nd point to form rectangle
options?	RectOptionsType		(optional) - Object with optional parameters: isCentered - a flag which defines if the rectangle is created as centered or not; fixation - a flag which defines if fixation constraints should be autogenerated or not; incidence - a flag which defines if coincidence constraints should be autogenerated or not; tangency - a flag which defines if tangency constraints should be autogenerated or not;

Returns Promise<void>

createReferenceGeometry

Creates new "Use"-Geometry in sketch

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, referenceIds: ObjectID[]): Promise<ObjectID[] | null>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch to which the new geometry is appended
referenceIds	ObjectID[]		Ids of the CC_Arc/Circle/Line/Point or edge or vertex

Returns Promise<ObjectID[] | null>
The array of ids of the new created objects or null.

createRigidSet

Adds rigid set to sketch

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, selectedObjs: ObjectID[]): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch
selectedObjs	ObjectID[]		Involved geometry objects

Returns Promise<void>

createSketch

Create a new sketch on the only existing part

Declaration

async (drawingId: DrawingID, partId: ObjectID): Promise<ObjectID | null>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
partId	ObjectID

Returns Promise<ObjectID | null>
The id of the new created sketch or null.

deleteFillet

Deleted a fillet by removing an arc and constraints and connecting lines

sketchId - id of the sketch arcId - id of the arc vertexId - id of the point in place of which filleted lines will be connected lineStartIds - array of ids of 2 points of filleted lines which are conneted with an arc constraintIds - array of ids of constraints which should have their entities replaced

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, arcId: ObjectID, vertexId: ObjectID, lineStartIds: ObjectID[], constraintIds: ObjectID[]): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID
sketchId	ObjectID
arcId	ObjectID
vertexId	ObjectID
lineStartIds	ObjectID[]
constraintIds	ObjectID[]

Returns Promise<void>

generateAutoConstraints

Automatically generates constraints whenever it makes sense and doesn't add up redundancy

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, objectId: ObjectID, autoConstr: autoConstrT): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch
objectId	ObjectID		Id of the object to autoconstrain (CC_Sketch id if need to autoconstraint each of its objects)
autoConstr	autoConstrT

Returns Promise<void>

loadSketch

Loads an ofb file from stream and copies the sketch elements from sketch with name = sketchName to the existing sketch with id = sketchId.

Declaration

async (drawingId: DrawingID, partId: ObjectID, sketchId: ObjectID, strm: ArrayBuffer, sketchName?: string): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
partId	ObjectID		Id of the part to load the sketch into
sketchId	ObjectID		Id of the sketch to copy elements from loaded sketch into it
strm	ArrayBuffer		Stream of the ofb file where we want to load a sketch from and copy its sketch elements
sketchName?	string		Optional name of the sketch to load from filestream, otherwise first sketch will be chosen

Returns Promise<void>

moveObjects

Translates objects in the delta direction

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, objectIds: ObjectID[], delta: PointMemValue): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch
objectIds	ObjectID[]		Array of objects to be translated
delta	PointMemValue		Direction of the translation

Returns Promise<void>

recalc

Recalculates geometry of the sketch

Declaration

async (drawingId: DrawingID, sketchId: ObjectID): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch

Returns Promise<void>

removeObjects

Removes objects from the sketch

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, objectIds: ObjectID[], storeState: boolean = true): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch
objectIds	ObjectID[]		Array of object ids to be removed from the sketch
storeState?	boolean	true	Optional flag for whether the state should be stored or not; true by default

Returns Promise<void>

setSketchRefs

Sets the references for sketch position

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, planeId: ObjectID | null, invertPlane: boolean, axisId: ObjectID | null, isXAxis: boolean, invertAxis: boolean, originId: ObjectID | null): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch to set the references
planeId	ObjectID l null		Id of a face or a workplane. This will be the plane where the sketch lies on
invertPlane	boolean		If true, the normal of the plane will be inverted
axisId	ObjectID l null		Id of an edge or workaxis. This will be the x-Axis
isXAxis	boolean		If true, the axisId will be the x-axis of the sketch, else the x-Axis will be the crossvector of the normal and the axisId
invertAxis	boolean		If true, the direction of the axis will be inverted
originId	ObjectID l null		Optional point or vertex of the sketch's origin reference

Returns Promise<void>

setWorkPlane

Sets selected workplane for the sketcher

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, planeId: ObjectID): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch
planeId	ObjectID		Id of the plane

Returns Promise<void>

solveConstraints

Solves all constraints.

Declaration

async (drawingId: DrawingID, sketchId: ObjectID): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch

Returns Promise<void>

splitAllCurves

Split all curves. Result of split - a container with new objects. After spliting splitCurvesMergeBack should be called.

Declaration

async (drawingId: DrawingID, sketchId: ObjectID): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch

Returns Promise<void>

splitCurves

Splits 1 or 2 curves in specified parameterized positions

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, curveIds: ObjectID[], paramArr: number[][]): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id
sketchId	ObjectID		Id of the sketch
curveIds	ObjectID[]		Array of 1 or 2 curve ids to be split
paramArr	number[][]		Array of 1 or 2 arrays (same length as curveIds array - so paramArr[0] has values for curveIds[0], paramArr[1] for curveIds[1], if it is defined), which consist of split parameter values (in range (0, 1)). Parameter value represents position on the curve from its start to the end (or from 0 to 2*PI for circles)

Returns Promise<void>

splitCurvesMergeBack

Merge splitted curves back.

Declaration

async (drawingId: DrawingID, sketchId: ObjectID): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch

Returns Promise<void>

unlinkReferenceGeometry

Unlinks "Use"-Geometry in sketch - geometry still exists but it is not connected to reference

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, useGeometryId: ObjectID): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch which the geometry belongs to
useGeometryId	ObjectID		Id of the CC_Arc/Circle/Line/Point that should be unlinked

Returns Promise<void>

updateDimensionValue

Updates value of constraint connected to dimension and recalculates sketch (SolveConstraints and UpdateDimensions)

Declaration

async (drawingId: DrawingID, dimensionId: ObjectID, value: APIParam<number>): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID
dimensionId	ObjectID		Id of the dimension
value	APIParam<number>		The new value or expression for dimension and constraint

Returns Promise<void>

updateDimensions

Updates sketch dimensions

Declaration

async (drawingId: DrawingID, sketchId: ObjectID): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch

Returns Promise<void>

updateGeometry

Updates sketch geometry

Declaration

async (drawingId: DrawingID, sketchId: ObjectID, geometryIds: ObjectID[], params: PointType | LineType | ArcType | CircleType): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
sketchId	ObjectID		Id of the sketch
geometryIds	ObjectID[]		Array of geometry object ids to be removed from the sketch
params	PointType l LineType l ArcType l CircleType		Parameter for a point, line, arc or circle.

Returns Promise<void>

updateSketchRegions

Updates multiple regions with new sets of curves

Declaration

async (drawingId: DrawingID, regionIds: ObjectID[], curvesArr: ObjectID[][]): Promise<void>

Params

Name	Type	Default	Description
drawingId	DrawingID		The drawing id.
regionIds	ObjectID[]		Array of ids of regions to be updated
curvesArr	ObjectID[][]		Array of arrays of curve ids; curvesArr[i] will be set as curves of regionIds[i] region

Returns Promise<void>