How to create a sketch break using the Fusion 360 API

[lukeQA94F]

Hi I'm wanting to break a spline with multiple fit points into multiple individual splines.

I can import the spline points from a csv, create the spline, add lines at every fit point so I can break the sketch up manually but I was wondering if there is a function to break the sketch using the fusion api, i.e <Sketch>.break(<3D_Point_1, <3D_Point_2>)

Cheers,

Luke

[kandennti]

Hi @lukeQA94F -San.

I tried to find it, but there seems to be no break function.
I tried to make a sample using the text command, but I don't think it is useful for actual use.

# Fusion360API Python script

import traceback
import adsk.core as core
import adsk.fusion as fusion


def run(context):
    ui: core.UserInterface = None
    try:
        app: core.Application = core.Application.get()
        ui = app.userInterface
        app.documents.add(core.DocumentTypes.FusionDesignDocumentType)

        des: fusion.Design = app.activeProduct
        root: fusion.Component = des.rootComponent

        ary = [
            [0, 0, 0],
            [1, 3, 0],
            [2, -1, 0],
            [3, 0, 0],
            [4, 2, 0],
            [5, 0, 0],
        ]
        points = [core.Point3D.create(*a) for a in ary]

        skt: fusion.Sketch = root.sketches.add(
            root.xYConstructionPlane
        )

        crv: fusion.SketchFittedSpline = create_spline(skt, points)

        break_curve_by_points(crv, points[1:-1])

    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))


def break_curve_by_points(
    crv: fusion.SketchEntity,
    points: list[core.Point3D],
):

    app: core.Application = core.Application.get()
    sels: core.Selections = app.userInterface.activeSelections

    skt: fusion.Sketch = crv.parentSketch

    target: fusion.SketchFittedSpline = crv
    for pnt in points:

        sels.clear()
        sels.add(skt)
        app.executeTextCommand(u"Commands.Start SketchActivate")

        target = break_curve(target, pnt)

        app.executeTextCommand(u"Commands.Start SketchStop")


def break_curve(
    crv: fusion.SketchEntity,
    point: core.Point3D,
):

    app: core.Application = core.Application.get()
    sels: core.Selections = app.userInterface.activeSelections

    eva: core.CurveEvaluator3D = crv.geometry.evaluator

    _, prm = eva.getParameterAtPoint(point)
    _, vec, _ = eva.getCurvature(prm)
    vec.scaleBy(0.01)

    sPnt: core.Point3D = point.copy()
    sPnt.translateBy(vec)

    vec.scaleBy(-1)
    ePnt: core.Point3D = point.copy()
    ePnt.translateBy(vec)

    skt: fusion.Sketch = crv.parentSketch
    lines: fusion.SketchLines = skt.sketchCurves.sketchLines
    tool: fusion.SketchLine = lines.addByTwoPoints(sPnt, ePnt)

    sels.clear()
    sels.add(crv)
    app.executeTextCommand(u"Commands.Start BreakSketchCmd")

    try:
        tool.deleteMe()
    except:
        pass

    sels.clear()

    return skt.sketchCurves[-1]


def create_spline(
    skt: fusion.Sketch,
    points: list[core.Point3D],
) -> fusion.SketchFittedSpline:

    splines: fusion.SketchFittedSplines = skt.sketchCurves.sketchFittedSplines
    return splines.add(
        core.ObjectCollection.createWithArray(points)
    )

[kandennti · Accepted solution]

@lukeQA94F -San.

Another idea is to use parameters to create a new curve for each interval and delete the original curve.

# Fusion360API Python script

import traceback
import adsk.core as core
import adsk.fusion as fusion


def run(context):
    ui: core.UserInterface = None
    try:
        app: core.Application = core.Application.get()
        ui = app.userInterface
        app.documents.add(core.DocumentTypes.FusionDesignDocumentType)

        des: fusion.Design = app.activeProduct
        root: fusion.Component = des.rootComponent

        ary = [
            [0, 0, 0],
            [1, 3, 0],
            [2, -1, 0],
            [3, 0, 0],
            [4, 2, 0],
            [5, 0, 0],
        ]
        points = [core.Point3D.create(*a) for a in ary]

        skt: fusion.Sketch = root.sketches.add(
            root.xYConstructionPlane
        )

        crv: fusion.SketchFittedSpline = create_spline(skt, points)

        create_split_curve_by_points(crv, points)

    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))


def create_split_curve_by_points(
    crv: fusion.SketchEntity,
    points: list[core.Point3D],
    removeOriginal: bool = True,
):
    geo = crv.geometry
    nurbs: core.NurbsCurve3D = None
    if hasattr(geo, "asNurbsCurve"):
        nurbs = geo.asNurbsCurve
    else:
        nurbs = geo

    eva: core.CurveEvaluator3D = nurbs.evaluator
    _, prms = eva.getParametersAtPoints(points)

    crvs = [nurbs.extract(s, e) for s, e in zip(prms, prms[1:])]

    skt: fusion.Sketch = crv.parentSketch
    splines: fusion.SketchFixedSplines = skt.sketchCurves.sketchFixedSplines

    [splines.addByNurbsCurve(c) for c in crvs]

    if removeOriginal:
        crv.deleteMe()


def create_spline(
    skt: fusion.Sketch,
    points: list[core.Point3D],
) -> fusion.SketchFittedSpline:

    splines: fusion.SketchFittedSplines = skt.sketchCurves.sketchFittedSplines
    return splines.add(
        core.ObjectCollection.createWithArray(points)
    )

[Jorge_Jaramillo · Accepted solution]

@Jorge_Jaramillo - this post is being edited to remove PII.

Hi @lukeQA94F ,

I was able to split the curve with the spline's built-in function breakCurve().

Here is the code:

def break_spline():
    points = [(0,0,0), (5,-1,0), (6,4,0), (2,5,0), (-1,2,0)]
    oc = adsk.core.ObjectCollection.create()
    for coords in points:
        oc.add(adsk.core.Point3D.create(*coords))

    # gets first sketch on root's current desing
    skt = root.sketches[0]

    # creates spline with the points provided
    sfs = skt.sketchCurves.sketchFittedSplines.add(oc)
    sfs.isClosed = True

    # print lines on the sketch
    app.log('Before splitting:')
    for i in range(skt.sketchCurves.count):
        app.log(f'      {i}   {skt.sketchCurves[i]}')

    # make n-1 curve breaks
    for i in range(len(points)-1):
        # make a circle intersecting the curve in points i-th and (i+1)-th
        sk_c = skt.sketchCurves.sketchCircles.addByTwoPoints(oc[i], oc[i+1])
        # get a point before and near the (i+1)-th point
        #
        # it has to be different that the intersecting point, so that is why it is multiplied by 90%
        #
        (_, par) = sfs.geometry.evaluator.getParameterAtPoint(oc[i+1])
        par *= 0.9
        (_, po_break) = sfs.geometry.evaluator.getPointAtParameter(par)
        # then break the curve using that point
        ocr = sfs.breakCurve(po_break)

        # delete the circle
        sk_c.deleteMe()

        # look for the original spline in the sketchFittedSplines collection
        #  I could NOT use the endSketchPoint attribute because it generates an exception
        #  (it is possible a BUG!! since every spline has to contain an endSketchPoint)
        for sfs_i in range(skt.sketchCurves.sketchFittedSplines.count):
            if skt.sketchCurves.sketchFittedSplines[sfs_i].fitPoints.count:
               fitPoints = skt.sketchCurves.sketchFittedSplines[sfs_i].fitPoints.count
               if skt.sketchCurves.sketchFittedSplines[sfs_i].fitPoints[fitPoints-1].geometry.isEqualTo(oc[0]):
                   sfs = skt.sketchCurves.sketchFittedSplines[sfs_i]
                   break

    # print lines on the sketch
    app.log('After splitting:')
    for i in range(skt.sketchCurves.count):
        app.log(f'      {i}   {skt.sketchCurves[i]}')

After breaking the spline I experienced some errors trying to access start and end points of the result splines, which could be a bug in the product.  That is the reason to check for fitpoints (line #40 in the code above) count first instead of the endSketchPoint attribute.

I hope this could help.

Regards,

Jorge Jaramillo

[lukeQA94F]

Cheers @kandennti and @Jorge_Jaramillo , both your solutions worked! Thanks for your help