Sketch

create(param)

Creates a new sketch and places it optionally on a face or work plane

if planeId is a face, a new work plane on that face will be created
if planeId is a workplane, the sketch will directly placed on it

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: id|VOID  // id of the new sketch
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the part to create the sketch on
[param.planeId]	`string` \| `real` \| `id`	id of the face or work plane to place the sketch on

Example

res = api.v1.sketch.create({ id: 4 })
res = api.v1.sketch.create({ id: 4, planeId: 15 })

setWorkPlane(param)

Sets workplane for the sketch

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to set workplane for
param.planeId	`string` \| `real` \| `id`	id of the work plane to set the sketch on

Example

res = api.v1.sketch.setWorkPlane({ id: 4, planeId: 15 })

constraint(param)

Creates one or multiple constraints in the sketch

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: id|VOID|Array<id|VOID>  // id or ids of created constraints
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object` \| `Array<object>`	object or objects containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to create constraints in
[param.name]	`string`	name of the constraint to create
param.type	`"COINCIDENT"` \| `"COLINEAR"` \| `"CONCENTRIC"` \| `"EQUAL_LENGTH"` \| `"EQUAL_RADIUS"` \| `"FIXATION"` \| `"HORIZONTAL"` \| `"MIDPOINT"` \| `"PARALLEL"` \| `"PERPENDICULAR"` \| `"SPLINE_FIT_POINT"` \| `"SYMMETRY"` \| `"TANGENT"` \| `"VERTICAL"`	type of the constraint to create
param.geomIds	`Array<(string\|real\|id)>`	sketch geometry like points, curves, ... which will be constrained

Example

res = api.v1.sketch.constraint({ id: 796, type: 'HORIZONTAL', geomIds: [startPt, endPt] })
res = api.v1.sketch.constraint({ id: 796, type: 'VERTICAL', geomIds: [line3] })
res = api.v1.sketch.constraint({ id: 796, name: 'A', type: 'COINCIDENT', geomIds: [873, 875] })

dimension(param)

Creates one or multiple dimensional constraints in the sketch

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: id|VOID|Array<id|VOID>  // id or ids of created dimensional constraints
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Default	Description
param	`object` \| `Array<object>`		object or objects containing all the parameters
param.id	`string` \| `real` \| `id`		id of the sketch to create dimensional constraints in
[param.name]	`string`		name of the constraint to create
param.type	`"RADIUS"` \| `"DIAMETER"` \| `"OFFSET"` \| `"HORIZONTAL_DISTANCE"` \| `"VERTICAL_DISTANCE"` \| `"ANGLE"` \| `"ANGLEOX"`		type of the constraint to create
[param.value]	`real` \| `expression`		value or expression to set for this dimensional constraint. If empty, value will be calculated automatically
param.geomIds	`Array<(string\|real\|id)>`		sketch geometry like points, curves, ... which will be constrained
[param.dimPos]	`point`		position of the dimension text, in case of type is "ANGLE", it also can be used to define which sector to be constrained
[param.reflex]	`boolean`	`FALSE`	If true, the angle will be the reflex angle in case of type is "ANGLE", which is bigger than 180deg, actually the outside angle (default=FALSE)

Example

res = api.v1.sketch.dimension({ id: sketch, type: 'ANGLE', geomIds: [873, 875], dimPos: [45, 80, 0], value: '60g' })
res = api.v1.sketch.dimension({ id: sketch, type: 'OFFSET', geomIds: [res.startId, res.endId] })

sketchRegion(param)

Creates a sketch region for a given sketch from sketch geometry

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: id  // id of the created sketch region
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to create the sketch region
[param.name]	`string`	name of the sketch region
param.geomIds	`Array<(string\|real\|id)>`	sketch geometry that the new sketch region will consist of, all should belong to the given sketch

Example

res = api.v1.sketch.sketchRegion({ id: 796, geomIds: [852, 863, 895, 912] })

changeReferenceGeometry(param)

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

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch which the geometry belongs to
param.geomId	`string` \| `real` \| `id`	id of the sketch geometry that should be relinked
param.refId	`string` \| `real` \| `id`	id of the new brep element to be referenced, like edge or vertex

Example

res = api.v1.sketch.changeReferenceGeometry({ id: 12, geomId: 56, refId: 85 })

circularPattern(param)

Patterns a rigidset (or single object) in circular arrange/order

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: {
     constraint: id,
     dimension: id|VOID,
     geometry: Array<id>
  }
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to create circular pattern in
param.rigidSetId	`string` \| `real` \| `id`	id of the rigid set to pattern
param.centerId	`string` \| `real` \| `id`	id of the point to be used as an origin for rotation
param.angle	`real`	angular offset in radians between neighbouring patterned objects around rotation center
param.count	`real`	number of copies

Example

res = api.v1.sketch.circularPattern({ id: 42, rigidSetId: 60, centerId: 61, angle: 90g, count: 4 })

mirrorPattern(param)

Patterns a rigidset (or single object) in mirror arrange/order

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: {
     constraint: id,
     geometry: Array<id>
  }
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to create mirror pattern in
param.rigidSetId	`string` \| `real` \| `id`	id of the rigid set to pattern
param.symmetryLineId	`string` \| `real` \| `id`	id of the line to be used as a symmetry line

Example

res = api.v1.sketch.mirrorPattern({ id: 42, rigidSetId: 60, symmetricLineId: 61 })

copyGeometry(param)

Copies sketch geometry

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: id[]|VOID  // ids of copied objects
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Default	Description
param	`object`		object containing all the parameters
param.id	`string` \| `real` \| `id`		id of the sketch to copy object
param.geomIds	`string` \| `real` \| `id`		ids of the sketch geometry to copy
param.translation	`point`		offset from initial objects as translation vector
[param.doCopyConstraints]	`boolean`	`TRUE`	a flag allowing to restrict copying constraints from original selected objects (default=TRUE)

Example

res = api.v1.sketch.copyGeometry({ id: 6, geomIds: [25, 36, 47, 58], translation: [20, 30, 0] })

linearPattern(param)

Patterns a rigidset (or single object) in linear/rectangular arrange/order. Copy count number over at least one dimension should be specified.

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: {
     constraint: id,
     dimensions: Array<id|VOID>,
     geometry: Array<id>
  }
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Default	Description
param	`object`		object containing all the parameters
param.id	`string` \| `real` \| `id`		id of the sketch to create linear pattern in
param.rigidSetId	`string` \| `real` \| `id`		id of the rigid set to pattern
[param.xDistance]	`real`	`0`	horizontal offset (x-axis) between neighbouring patterned objects (default=0)
[param.yDistance]	`real`	`0`	vertical offset (y-axis) between neighbouring patterned objects (default=0)
[param.xCount]	`real`	`1`	number of copies along the x-axis (default=1)
[param.yCount]	`real`	`1`	number of copies along the y-axis (default=1)

Example

res = api.v1.sketch.linearPattern({ id: 42, rigidSetId: 60, xCount: 5, xDistance: 30 })
res = api.v1.sketch.linearPattern({ id: 42, rigidSetId: 60, xCount: 3, xDistance: 50, yCount: 3, yDistance: 100 })

copyFrom(param)

Copies the sketch geometry from one sketch to another

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the existing sketch to copy sketch geometry into it
param.toCopyId	`string` \| `real` \| `id`	id of the sketch to copy elements from

Example

res = api.v1.sketch.copyFrom({ id: 6, toCopyId: 25 })

fillet(param)

Creates a fillet in place of a point and its connecting two lines

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: Array<id>|VOID  // a tuple of (arcId, controlPointId, startPointId, endPointId) or VOID if fillet couldn't be created
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to create the fillet in
param.lineIds	`Array<(string\|real\|id)>`	ids of the two lines to create the fillet at its connecting point
[param.offset]	`real`	offset from the incidence point to fillet arc start / end. If neither param.offset or param.radius are set, param.offset is taken 1/4 length of the shortest of lines referred in param.lineIds
[param.radius]	`real`	radius of the fillet arc. Is ignored if param.offset is set

Example

res = api.v1.sketch.fillet({ id: 6, lineIds: [15, 18], offset: 10 })
res = api.v1.sketch.fillet({ id: 6, lineIds: [15, 18], radius: 8 })

rectangle(param)

Creates a rectangle formed by two positions

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: Array<id>  // ids of the lines of the created rectangle
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

result information:

index 0: horizontal line not connected to end position
index 1: vertical line connected to end position
index 2: horizontal line connected to end position
index 3: vertical line not connected to end position

Param	Type	Default	Description
param	`object`		object containing all the parameters
param.id	`string` \| `real` \| `id`		id of the sketch to create the rectangle in
param.startPos	`point`		position of the first point to form the rectangle
param.endPos	`point`		position of the second point to form the rectangle
[param.isCentered]	`boolean`	`FALSE`	a flag which defines if the rectangle is created as centered or not (default=FALSE)
[param.genFixation]	`boolean`	`TRUE`	a flag which defines if fixation in the Origin should be autogenerated or not (default=TRUE)
[param.genIncidence]	`boolean`	`TRUE`	a flag which defines if coincidence constraints between an existing point and the new rectangle corner should be autogenerated or not (default=TRUE)
[param.genTangency]	`boolean`	`TRUE`	a flag which defines if tangency constraints between an existing arc and new rectangle should be autogenerated or not (default=TRUE)

Example

res = api.v1.sketch.rectangle({ id: 6, startPos: [0, 0, 0], endPos: [20, 20, 0], isCentered: TRUE })

referenceGeometry(param)

Creates new "Use"-Geometry in sketch. The sketch geometry will be created at the given brep elements and projected into sketch plane. It also creates a reference to the given brep element.

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to create the reference geometry in
param.brepIds	`string` \| `real` \| `id`	ids of the brep elements to create sketch geometry at and reference on

Example

res = api.v1.sketch.referenceGeometry({ id: 6, brepIds: [256, 258, 236] })

rigidSet(param)

Creates a rigid set from given sketch geometry in the sketch

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: id|VOID  // id of the created rigid set
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to create the rigid set in
param.geomIds	`Array<(string\|real\|id)>`	ids of sketch geometry to create the rigid set from

Example

res = api.v1.sketch.rigidSet({ id: 6, geomIds: [25, 28, 31, 33] })

undoFillet(param)

Deletes an existing fillet by removing the arc and its constraints and connect lines again

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to delete the fillet in
param.arcId	`string` \| `real` \| `id`	id of the fillet-made arc to delete

Example

res = api.v1.sketch.undoFillet({ id: 6, arcId: 89 })

generateAutoConstraints(param)

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

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Default	Description
param	`object`		object containing all the parameters
param.id	`string` \| `real` \| `id`		id of the sketch to generat auto constraints
param.geomId	`string` \| `real` \| `id`		id of the sketch geometry to auto constraint or the sketch id itself to autoconstraint each of sketch's objects
[param.genFixation]	`boolean`	`TRUE`	a flag which defines if fixation in the Origin should be autogenerated or not (default=TRUE)
[param.genIncidence]	`boolean`	`TRUE`	a flag which defines if coincidence constraints between an existing point and the new rectangle corner should be autogenerated or not (default=TRUE)
[param.genTangency]	`boolean`	`TRUE`	a flag which defines if tangency constraints between an existing arc and new rectangle should be autogenerated or not (default=TRUE)
[param.genVertAndHoriz]	`boolean`	`TRUE`	a flag which defines if vertical and horizontal constraints should be autogenerated or not (default=TRUE)

Example

res = api.v1.sketch.generateAutoConstraints({ id: 6, geomId: 56 })

loadFrom(param)

Loads an ofb file by filename, data or url and copies the sketch geometry from loaded sketch to the existing sketch

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Default	Description
param	`object`		object containing all the parameters
param.id	`string` \| `real` \| `id`		id of the sketch to copy sketch elements into it
param.partId	`string` \| `real` \| `id`		id of the part to load the sketch into
[param.url]	`string`		url to loading ofb file, where the sketch want be loaded from
[param.file]	`string`		full path of the file. Path has to be a for the ClassCAD process reachable local or UNC path.
[param.data]	`string`		data/content of the model to load sketch from
[param.encoding]	`"base64"`		the encoding the data is encoded with. If compression is also set, the decoding happens first!
[param.compression]	`"deflate"`		the compression algorithm the data is compressed with.
[param.format]	`"OFB"`	`"OFB"`	content format of to load file, where the sketch want to be loaded from (default="OFB")
[param.name]	`string`		name of the sketch in the loaded ofb file, if no name is given, the first found sketch will be chosen

Example

res = api.v1.sketch.loadFrom({ id: 6, partId: 69, url: 'https://.../file.ofb', format: 'ofb' })
res = api.v1.sketch.loadFrom({ id: 6, partId: 69, file: '/var/models/file.ofb' })
res = api.v1.sketch.loadFrom({ id: 6, partId: 69, data: 'xx124b', format: 'ofb' })

moveGeometry(param)

Moves the given sketch geometry by translation vector

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: boolean  // true if sketch state is still solved
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to move sketch geometry in
param.geomIds	`Array<(string\|real\|id)>`	ids of the sketch geometry to move by translation vector
param.translation	`point`	translation vector to move sketch geometry

Example

res = api.v1.sketch.moveGeometry({ id: 6, geomIds: [45, 58], translation: [20, 85, 0] })

setReferences(param)

Creates and sets the plane, axis and origin reference of the sketch

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Default	Description
param	`object`		object containing all the parameters
param.id	`string` \| `real` \| `id`		id of the sketch to set the references
[param.planeId]	`string` \| `real` \| `id`		id of a face or a workplane. This will be the plane where the sketch lies on.
[param.invertPlane]	`boolean`	`FALSE`	if true, the normal of the plane will be inverted (default=FALSE)
[param.axisId]	`string` \| `real` \| `id`		id of a line or a workaxis.
[param.isXAxis]	`boolean`	`TRUE`	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 (default=TRUE)
[param.invertAxis]	`boolean`	`FALSE`	if true, the direction of the axis will be inverted (default=FALSE)
[param.originId]	`string` \| `real` \| `id`		id of a point or vertex of the sketch's origin reference

Example

res = api.v1.sketch.setReferences({ id: 6, planeId: 58 })

splitAllCurves(param)

Splits all curves in the given sketch

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: Array<id|VOID> // Array of trimmable curves
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to split all curves

Example

res = api.v1.sketch.splitAllCurves({ id: 6 })

splitCurves(param)

Splits curves in specified parameterized positions

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID|Array<Array<id|VOID>>
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

result information:

VOID is returned if it isn't possible to split one or more specified entities.
Otherwise, an array of same length as param.splits is returned.
It contains arrays of ids of splitted curves in the same order as in param.splits.
If the length of param.splits[i] was N, then the length of result[i] will be N+1.

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to split curves
param.splits	`Array<object>`	objects containing the split information
param.splits.geomId	`string` \| `real` \| `id`	id of curve to be split
param.split.values	`Array<real>`	split values for the curve to be split. values are in range of [0,1]. value represents position on the curve from its start to the end (or from 0 to 2*PI for circles)

Example

res = api.v1.sketch.splitCurves({ id: 6, splits: [{ geomId: 25, values: [0.236, 0.82345124] }] })

splitCurvesMergeBack(param)

Merges the splitted curves back

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to merge back splitted curves

Example

res = api.v1.sketch.splitCurvesMergeBack({ id: 6 })

unlinkReferenceGeometry(param)

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

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to unlink referenced sketch geometry
param.geomId	`string` \| `real` \| `id`	id of the sketch geometry to unlink

Example

res = api.v1.sketch.unlinkReferenceGeometry({ id: 6, geomId: 48 })

updateDimension(param)

Updates the dimension of sketch geometry and recalculates the sketch

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: boolean  // true if sketch state is solved
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the dimension to update
param.value	`real` \| `expression`	the new value or expression for the dimension

Example

res = api.v1.sketch.updateDimension({ id: 256, value: 50 })
res = api.v1.sketch.updateDimension({ id: 256, value: '@expr.distance1' })

updateGeometry(param)

Updates the sketch geometry

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Default	Description
param	`object`		object containing all the parameters
param.id	`string` \| `real` \| `id`		id of the sketch to update sketch geometry
[param.points]	`Array<object>`		array of points to create
param.points[].id	`point`		id of the point to update
param.points[].pos	`point`		new position of the point
[param.lines]	`Array<object>`		array of lines to create
param.lines[].id	`point`		id of the line to update
param.lines[].startPos	`point`		new start position of the line
param.lines[].endPos	`point`		new end position of the line
[param.arcsBy3Points]	`Array<object>`		array of arcs to create by three given points
param.arcsBy3Points[].id	`point`		id of the arc to update by 3 points
param.arcsBy3Points[].startPos	`point`		start position of the arc
param.arcsBy3Points[].endPos	`point`		end position of the arc
param.arcsBy3Points[].midPos	`point`		middle position on the arc (not center)
[param.arcsByCenter]	`Array<object>`		array of arcs to create by start-, end- and center point
param.arcsByCenter[].id	`point`		id of the arc to update by center
param.arcsByCenter[].startPos	`point`		start position of the arc
param.arcsByCenter[].endPos	`point`		end position of the arc
param.arcsByCenter[].centerPos	`point`		center position of the arc
[param.arcsByCenter[].isClockwise]	`boolean`	`TRUE`	flag to define whether the arc is clockwise from start- to end-point around center-point or not (default=TRUE)
[param.circles]	`Array<object>`		array of circles to create
param.circles[].id	`point`		id of the circle to update
param.circles[].centerPos	`point`		center position of the circle
param.circles[].radius	`real`		radius of the circle

Example

res = api.v1.sketch.updateGeometry({ id: 6, points: [{ id: 25, pos: [10,50,0], { id: 29, pos: [10,60,0] }] })
res = api.v1.sketch.updateGeometry({ id: 6, circles: [{ id: 56, centerPos: [40,50,0], radius: 15 }] })

updateSketchRegion(param)

Updates sketch regions with new sketch geometry

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.regions	`Array<object>`	array of objects containing update informaton for the region
param.regions.id	`string` \| `real` \| `id`	id of the sketch region to update
param.regions.geomIds	`Array<(string\|real\|id)>`	array or sketch geometry to update the region with

Example

res = api.v1.sketch.updateSketchRegion({ id: 79, regions: [{ id: 45, geomIds: [14, 78, 96] }] })

getPoints(param)

Get the specific point ids of lines, arcs or circles

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: { startId: string|real|id, endId: string|real|id } |
     { startId: string|real|id, endId: string|real|id, centerId: string|real|id } |
     { centerId: string|real|id } |
     VOID  // object containing the specific points, which define the geometry which has been provided
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

result information:

if input is a line then it returns an object containing startId and endId of the line
if input is an arc then it returns an object containing startId, endId and centerId of the arc
if input is a circle then it returns an object containing centerId of the circle

Param	Type	Description
param	`object`	object containing the parameters
param.id	`string` \| `real` \| `id`	id of the geometry (e.g. line, arc, circle) to get the specific point ids from

Example

res = api.v1.sketch.getPoints({ id: 24 })

getPositions(param)

Get the specific positions of points, lines, arcs or circles

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: { pos: point } |
     { startPos: point, endPos: point } |
     { startPos: point, endPos: point, centerPos: point } |
     { centerPos: point } |
     VOID  // object containing the specific positions
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

result information:

if input is a point then it returns an object containing position of the point
if input is a line then it returns an object containing start- and end-position of the line
if input is an arc then it returns an object containing start-, end- and center-position of the arc
if input is a circle then it returns an object containing center-position of the circle

Param	Type	Description
param	`object`	object containing the parameters
param.id	`string` \| `real` \| `id`	id of the geometry (e.g. point, line, arc, circle) to get the specific positions from

Example

res = api.v1.sketch.getPoints({ id: 24 })

point(param)

Creates one or multiple points in the sketch

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: id|VOID|Array<id|VOID>  // id or ids of the added points
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Default	Description
param	`object` \| `Array<object>`		object or objects containing all the parameters
param.id	`string` \| `real` \| `id`		id of the sketch
param.pos	`point`		position of the point
[param.genFixation]	`boolean`	`TRUE`	a flag which defines if fixation in the Origin should be autogenerated or not (default=TRUE)
[param.genIncidence]	`boolean`	`TRUE`	a flag which defines if coincidence constraints between an existing and the new point should be autogenerated or not (default=TRUE)

Example

res = api.v1.sketch.point({ id: 42, pos: [0, 0, 0] })

line(param)

Creates one or multiple lines in the sketch

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: id|VOID|Array<id|VOID>  // id or ids of the added lines
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Default	Description
param	`object` \| `Array<object>`		object or objects containing all the parameters
param.id	`string` \| `real` \| `id`		id of the sketch
param.startPos	`point`		start position of the line
param.endPos	`point`		end position of the line
[param.genFixation]	`boolean`	`TRUE`	a flag which defines if fixation in the Origin should be autogenerated or not (default=TRUE)
[param.genIncidence]	`boolean`	`TRUE`	a flag which defines if coincidence constraints between an existing and the new point should be autogenerated or not (default=TRUE)
[param.genTangency]	`boolean`	`TRUE`	a flag which defines if tangency constraints between an existing curve and the new line should be autogenerated or not (default=TRUE)
[param.genVertAndHoriz]	`boolean`	`TRUE`	a flag which defines if vertical and horizontal constraints should be autogenerated or not (default=TRUE)

Example

res = api.v1.sketch.line({ id: 42, startPos: [0, 0, 0], endPos: [10, 10, 0] })

circle(param)

Creates one or multiple circles in the sketch

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: id|VOID|Array<id|VOID>  // id or ids of the added circles
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Default	Description
param	`object` \| `Array<object>`		object or objects containing all the parameters
param.id	`string` \| `real` \| `id`		id of the sketch
param.centerPos	`point`		center position of the circle
param.radius	`real`		radius of the circle
[param.genFixation]	`boolean`	`TRUE`	a flag which defines if fixation in the origin should be autogenerated or not (default=TRUE)
[param.genIncidence]	`boolean`	`TRUE`	a flag which defines if coincidence constraints between an existing and the new point should be autogenerated or not (default=TRUE)

Example

res = api.v1.sketch.circle({ id: 42, centerPos: [40, 0, 0], radius: 20 })

getGeometry(param)

Get all the sketch geometry from a sketch, sketch region or rigid set

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: { points: id[], lines: id[], arcs: id[], circles: id[] }  // object containing the sketch geometry
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing the parameters
param.id	`string` \| `real` \| `id`	id of the sketch, sketch region or rigid set

Example

res = api.v1.sketch.getGeometry({ id: 6 })

arcByCenter(param)

Creates one or multiple arcs by center in the sketch. Arc is defined by start-, end- and center-position.

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: id|VOID|Array<id|VOID>  // id or ids of the added arcs
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Default	Description
param	`object` \| `Array<object>`		object or objects containing all the parameters
param.id	`string` \| `real` \| `id`		id of the sketch
param.startPos	`point`		start position of the arc
param.endPos	`point`		end position of the arc
param.centerPos	`point`		center position of the arc
[param.isClockwise]	`boolean`	`TRUE`	flag to define whether the arc is clockwise from start- to end-point around center-point or not (default=TRUE)
[param.genFixation]	`boolean`	`TRUE`	a flag which defines if fixation in the origin should be autogenerated or not (default=TRUE)
[param.genIncidence]	`boolean`	`TRUE`	a flag which defines if coincidence constraints between an existing and the new point should be autogenerated or not (default=TRUE)

Example

res = api.v1.sketch.arcByCenter({ id: 42, startPos: [-40, 0, 0], centerPos: [0, 10, 0], endPos: [40, 0, 0] })

arcBy3Points(param)

Creates one or multiple arcs by 3 points in the sketch. Arc is defined by start-, end- and mid-position.

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: id|VOID|Array<id|VOID>  // id or ids of the added arcs
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Default	Description
param	`object` \| `Array<object>`		object or objects containing all the parameters
param.id	`string` \| `real` \| `id`		id of the sketch
param.startPos	`point`		start position of the arc
param.endPos	`point`		end position of the arc
param.midPos	`point`		middle position on the arc
[param.genFixation]	`boolean`	`TRUE`	a flag which defines if fixation in the origin should be autogenerated or not (default=TRUE)
[param.genIncidence]	`boolean`	`TRUE`	a flag which defines if coincidence constraints between an existing and the new point should be autogenerated or not (default=TRUE)

Example

res = api.v1.sketch.arcBy3Points({ id: 42, startPos: [0, 0, 0], midPos: [20, 20, 0], endPos: [40, 0, 0] })

geometry(param)

Creates one or multiple sketch geometry in the sketch

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: { points: id[], lines: id[], arcsBy3Points: id[],
     arcsByCenter: id[], circles: id[] }  // object containing created sketch geometry in the order of input
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Default	Description
param	`object`		object containing all the parameters
param.id	`string` \| `real` \| `id`		id of the sketch
[param.points]	`Array<object>`		array of points to create
param.points[].pos	`point`		position of the point
[param.lines]	`Array<object>`		array of lines to create
param.lines[].startPos	`point`		start position of the line
param.lines[].endPos	`point`		end position of the line
[param.arcsBy3Points]	`Array<object>`		array of arcs to create by three given points
param.arcsBy3Points[].startPos	`point`		start position of the arc
param.arcsBy3Points[].endPos	`point`		end position of the arc
param.arcsBy3Points[].midPos	`point`		middle position on the arc (not center)
[param.arcsByCenter]	`Array<object>`		array of arcs to create by start-, end- and center point
param.arcsByCenter[].startPos	`point`		start position of the arc
param.arcsByCenter[].endPos	`point`		end position of the arc
param.arcsByCenter[].centerPos	`point`		center position of the arc
[param.arcsByCenter[].isClockwise]	`boolean`	`TRUE`	flag to define whether the arc is clockwise from start- to end-point around center-point or not (default=TRUE)
[param.circles]	`Array<object>`		array of circles to create
param.circles[].centerPos	`point`		center position of the circle
param.circles[].radius	`real`		radius of the circle
[param.genFixation]	`boolean`	`TRUE`	a flag which defines if fixation in the Origin should be autogenerated or not (default=TRUE)
[param.genIncidence]	`boolean`	`TRUE`	a flag which defines if coincidence constraints between an existing point and the new point should be autogenerated or not (default=TRUE)
[param.genTangency]	`boolean`	`TRUE`	a flag which defines if tangency constraints between an existing curve and the new curve should be autogenerated or not (default=TRUE)
[param.genVertAndHoriz]	`boolean`	`TRUE`	a flag which defines if vertical and horizontal constraints should be autogenerated or not (default=TRUE)

Example

res = api.v1.sketch.geometry({ id: 42, points: [{ pos: [0,0,0] }, { pos: [10,10,0] }, { pos: [20,0,0]}] });
res = api.v1.sketch.geometry({ id: 42, lines: [{ startPos: [0,0,0], endPos: [0,20,0] }] );
res = api.v1.sketch.geometry({ id: 42, arcsBy3Points: [{ startPos: [0,20,0], endPos: [20,20,0], midPos: [10,30,0] }] );
res = api.v1.sketch.geometry({ id: 42, arcsByCenter: [{ startPos: [0,20,0], endPos: [20,20,0], centerPos: [10,20,0], isClockwise: FALSE }] );
res = api.v1.sketch.geometry({ id: 42, circles: [{ centerPos: [0,20,0], radius: 20 }, { centerPos: [0,40,0], radius: 10 }] );

deleteObject(param)

Deletes dimensions, constraints, sketch geometry, sketch region or rigid sets from sketch

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.ids	`Array<(string\|real\|id)>`	ids to delete

Example

res = api.v1.sketch.deleteObject({ ids: [15, 25, 23] })

deleteSketch(param)

Deletes existing sketches

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.ids	`string` \| `real` \| `id`	ids of the sketches to delete

Example

res = api.v1.sketch.deleteSketch({ ids: [6, 8] })

getSketchRegion(param)

Returns the id of the sketch region with the given name which belongs to the given sketch id.

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: id|VOID  // id of the found sketch region
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch to get the sketch region from
param.name	`string`	the name of the sketch region to look for

Example

res = api.v1.sketch.getSketchRegion({ id: 40, name: 'SketchRegion_Left' })

trimCurves(param)

Trims away curves, if they are suitable for trimming

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the sketch with curves to be trimmed away
param.curveIds	`Array<(string\|real\|id)>`	ids of sketch curves to be trimmed away

Example

res = api.v1.sketch.trimCurves({ id: 40, curveIds: [94, 100, 106] })

updateDimensionPosition(param)

Updates the position of the dimension text

Kind: v1.sketch function
Returns: object - object containing result and optional messages

{
  result: VOID
  messages?: { message: string, level: real, code: real, api: string }[]
  maxLevel?: real
}

Param	Type	Description
param	`object`	object containing all the parameters
param.id	`string` \| `real` \| `id`	id of the dimension to change the text position
param.pos	`point`	position of the dimension text to update

Example

res = api.v1.sketch.updateDimensionPosition({ id: 796, pos: [50, 60, 0] })

create(param)​

setWorkPlane(param)​

constraint(param)​

dimension(param)​

sketchRegion(param)​

changeReferenceGeometry(param)​

circularPattern(param)​

mirrorPattern(param)​

copyGeometry(param)​

linearPattern(param)​

copyFrom(param)​

fillet(param)​

rectangle(param)​

referenceGeometry(param)​

rigidSet(param)​

undoFillet(param)​

generateAutoConstraints(param)​

loadFrom(param)​

moveGeometry(param)​

setReferences(param)​

splitAllCurves(param)​

splitCurves(param)​

splitCurvesMergeBack(param)​

unlinkReferenceGeometry(param)​

updateDimension(param)​

updateGeometry(param)​

updateSketchRegion(param)​

getPoints(param)​

getPositions(param)​

point(param)​

line(param)​

circle(param)​

getGeometry(param)​

arcByCenter(param)​

arcBy3Points(param)​

geometry(param)​

deleteObject(param)​

deleteSketch(param)​

getSketchRegion(param)​

trimCurves(param)​

updateDimensionPosition(param)​

create(param)

setWorkPlane(param)

constraint(param)

dimension(param)

sketchRegion(param)

changeReferenceGeometry(param)

circularPattern(param)

mirrorPattern(param)

copyGeometry(param)

linearPattern(param)

copyFrom(param)

fillet(param)

rectangle(param)

referenceGeometry(param)

rigidSet(param)

undoFillet(param)

generateAutoConstraints(param)

loadFrom(param)

moveGeometry(param)

setReferences(param)

splitAllCurves(param)

splitCurves(param)

splitCurvesMergeBack(param)

unlinkReferenceGeometry(param)

updateDimension(param)

updateGeometry(param)

updateSketchRegion(param)

getPoints(param)

getPositions(param)

point(param)

line(param)

circle(param)

getGeometry(param)

arcByCenter(param)

arcBy3Points(param)

geometry(param)

deleteObject(param)

deleteSketch(param)

getSketchRegion(param)

trimCurves(param)

updateDimensionPosition(param)