Convert NURBS curve to Arc curve
Hi @miminguyenps1098 .
If a spline arc approximation is OK, I created it about 4 years ago.
# Fusion360API Python script
import traceback
import adsk.fusion
import adsk.core
# arc-approximation tolerance - Unit is Cm
tolerance = 0.001
def run(context):
ui = adsk.core.UserInterface.cast(None)
try:
app: adsk.core.Application = adsk.core.Application.get()
ui = app.userInterface
# 面選択
msg: str = 'Select curve/ESC-abort'
selFilter: str = 'SketchCurves'
sel: adsk.core.Selection = selectEnt(msg, selFilter)
if not sel:
return
crv = sel.entity
# 点群
points = initPointsOnCurve(crv.geometry, tolerance)
# 円弧近似
threeArcs = []
threeArcs = initThreePointArc(0, len(points)-1, tolerance, points, threeArcs)
if len(threeArcs) < 1:
ui.messageBox('Could not approximate the arc.')
return
# ｽｹｯﾁ作成
des = adsk.fusion.Design.cast(app.activeProduct)
comp = des.rootComponent
skt: adsk.fusion.Sketch = comp.sketches.add(comp.xYConstructionPlane)
skt.name = "ArcApproximation"
# 円弧作成
skt_arcs = skt.sketchCurves.sketchArcs
skt.isComputeDeferred = True
[skt_arcs.addByThreePoints(p1,p2,p3) for (p1,p2,p3) in threeArcs]
skt.isComputeDeferred = False
ui.messageBox(f'{len(threeArcs)} arc created')
except:
if ui:
ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
# 外心円
def getCircumCircleOFTraiangle(p1,p2,p3):
# 3点ベクトル取得
vec1_2 = adsk.core.Vector3D.cast(p2.asVector())
vec1_2.subtract(p1.asVector())
vec1_2.normalize()
vec2_3 = adsk.core.Vector3D.cast(p3.asVector())
vec2_3.subtract(p2.asVector())
vec2_3.normalize()
# 平行ﾁｪｯｸ
if vec1_2.isParallelTo(vec2_3):
return None
# P2_P3間 オイラー線
eulerLine = vec2_3.crossProduct(vec1_2.crossProduct(vec2_3))
eulerLine.normalize()
# 中間点
p1_2 = getMidPoint3D(p1,p2)
p2_3 = getMidPoint3D(p2,p3)
# 不明
nv = vec1_2.dotProduct(eulerLine)
t = (vec1_2.dotProduct(p1_2.asVector()) - vec1_2.dotProduct(p2_3.asVector())) / nv
# 外心
center = getCircumCenter(p2_3,eulerLine,t)
# 半径
radius = center.distanceTo(p1)
return (center, radius)
# 外心
def getCircumCenter(p,v,l):
pos = (p.x + v.x * l,
p.y + v.y * l,
p.z + v.z * l)
return adsk.core.Point3D.create(pos[0],pos[1],pos[2])
# 中間点
def getMidPoint3D(p1,p2):
pos = ((p1.x + p2.x) * 0.5,
(p1.y + p2.y) * 0.5,
(p1.z + p2.z) * 0.5)
return adsk.core.Point3D.create(pos[0],pos[1],pos[2])
def isInTolerance(center, radius, tol, points):
dist_lst = [radius - center.distanceTo(p) for p in points]
res = [d for d in dist_lst if d > tol]
return True if len(res) < 1 else False
# 3点円弧 再帰
def initThreePointArc(startIdx, endIdx, tol, points, threeArcs):
if 2 > (endIdx - startIdx):
return threeArcs
# 中間idx
midIdx = int((startIdx + endIdx) * 0.5)
arc = getCircumCircleOFTraiangle(
points[startIdx],
points[midIdx],
points[endIdx]
)
if arc is None:
return threeArcs
# 円弧評価
if isInTolerance(arc[0], arc[1], 0.001, points[startIdx+1:endIdx-1]):
threeArcs.append([points[startIdx],points[midIdx],points[endIdx]])
else:
threeArcs = initThreePointArc(startIdx, midIdx, tol, points, threeArcs)
threeArcs = initThreePointArc(midIdx, endIdx, tol, points, threeArcs)
return threeArcs
# トレランス以内の曲線上の点群
def initPointsOnCurve(geo, tol):
# evaluator
eva = geo.evaluator
# 始点終点
_, startPoint, endPoint = eva.getEndPoints()
_, startPram = eva.getParameterAtPoint(startPoint)
_, endPram = eva.getParameterAtPoint(endPoint)
# ﾄﾚﾗﾝｽ以内の点群
_, pnts = eva.getStrokes(startPram, endPram, tol)
return pnts
# 選択
def selectEnt(
msg: str,
filterStr: str) -> adsk.core.Selection:
try:
app = adsk.core.Application.get()
ui = app.userInterface
sel = ui.selectEntity(msg, filterStr)
return sel
except:
return None
Are you saying that you want to make a circular arc because originally one arc is a NURBS curve?
Attached is a NurbsCurve created from an arc.
Do you mean something like this?
If different, please attach a sample f3d file.
I do not understand English. Therefore, I cannot understand what you want even if you explain it only in words.
I told you beforehand to attach a sample f3d file if the f3d file I attached is different, but unfortunately you did not get the message.
I am not likely to be able to lend a hand.
Accepted solution
The CurveEvaluator3D object can be used to evaluate curves.
https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-GUID-dc7ae251-e060-4d87-b6b8-e7f78abc0777
I made a sample.
It examines the curvature at numerous positions on the curve, determines that if it is a constant value, it is an arc, and obtains the three points required for an arc.
# Fusion360API Python script
import traceback
import adsk.fusion
import adsk.core
def run(context):
ui = adsk.core.UserInterface.cast(None)
try:
app: adsk.core.Application = adsk.core.Application.get()
ui = app.userInterface
# select curve
msg: str = 'Select Sketch Curve'
selFilter: str = 'SketchCurves'
sel: adsk.core.Selection = selectEnt(msg, selFilter)
if not sel:
return
sktCrv: adsk.fusion.SketchCurve = sel.entity
# get ArcThreePoints
pnts = nurbs2ArcThreePoints(
sktCrv
)
if len(pnts) < 3:
ui.messageBox('Cannot be converted to a Arc')
return
# create Sketch
refSkt: adsk.fusion.Sketch = sktCrv.parentSketch
comp: adsk.fusion.Component = refSkt.parentComponent
skt: adsk.fusion.Sketch = comp.sketches.add(
refSkt.referencePlane
)
skt.name = 'Nurbs2Arc'
# create Arc
skt.sketchCurves.sketchArcs.addByThreePoints(
pnts[0],
pnts[1],
pnts[2],
)
ui.messageBox('Done')
except:
if ui:
ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
# return [Point3D,Point3D,Point3D]
def nurbs2ArcThreePoints(
sktCrv: adsk.fusion.SketchCurve,
tolerance: float = 0.001) -> list:
# line NG
if sktCrv.classType() == adsk.fusion.SketchLine.classType():
return []
# geometry
geo = sktCrv.geometry
# evaluator
eva: adsk.core.CurveEvaluator3D = geo.evaluator
# get Points On Curve
_, startPoint, endPoint = eva.getEndPoints()
_, startPrm = eva.getParameterAtPoint(startPoint)
_, endPrm = eva.getParameterAtPoint(endPoint)
_, pnts = eva.getStrokes(startPrm, endPrm, tolerance)
# get Parameters
_, prms = eva.getParametersAtPoints(pnts)
# get Curvatures
_, _, curvatures = eva.getCurvatures(prms)
curvatures = [round(v/tolerance)*tolerance for v in curvatures]
# Convertible or Evaluatable
if len(set(curvatures)) != 1:
return []
# Three points for Arc
return [
pnts[0],
pnts[len(pnts) // 2],
pnts[-1]
]
def selectEnt(
msg: str,
filterStr: str) -> adsk.core.Selection:
try:
app = adsk.core.Application.get()
ui = app.userInterface
sel = ui.selectEntity(msg, filterStr)
return sel
except:
return None
I have not looked into it, but it would probably be UnitsManager.internalUnits(Cm).
https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-7c2df7ad-aeea-49c1-96b5-71382f8d520f
Accepted solution
I'm a little late to the party, but hopefully, this will help. The script below prompts you to select a sketch curve. It uses the curve and the point you selected it at and compute the radius at the point and draws a line to the center of the radius of the curve at that location. It will work with any sketch curve, except for a line because it has infinite curvature.
Here's a picture after using the script on some test sketches.
def run(context):
ui = None
try:
app = adsk.core.Application.get()
ui = app.userInterface
design = adsk.fusion.Design.cast(app.activeProduct)
root = design.rootComponent
cg = root.customGraphicsGroups.add()
while True:
try:
skCurveSel = ui.selectEntity('Select a curve.', 'SketchCurves')
except:
cg.deleteMe()
app.activeViewport.refresh()
return
skCurve = skCurveSel.entity
worldGeom = skCurve.worldGeometry
eval = worldGeom.evaluator
(_, param) = eval.getParameterAtPoint(skCurveSel.point)
direction: adsk.core.Vector3D
(_, direction, curvature) = eval.getCurvature(param)
radius = 1/curvature
app.log(f'Curvature: {curvature}, Radius: {radius} cm')
pnt1 = skCurveSel.point
pnt2 = pnt1.copy()
direction.normalize()
direction.scaleBy(radius)
pnt1.translateBy(direction)
coords = list(pnt1.asArray())
coords.extend(list(pnt2.asArray()))
cgCoords = adsk.fusion.CustomGraphicsCoordinates.create(coords)
cg.addLines(cgCoords, [], False)
app.activeViewport.refresh()
except:
if cg:
cg.deleteMe()
app.activeViewport.refresh()
if ui:
ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
