topic Re: Sketching on one sketch for sweeping feature in Fusion API and Scripts Forum

Sketching on one sketch for sweeping feature

Anonymous — Sun, 05 Sep 2021 10:48:48 GMT

Hey,

Previously I was able to draw one full path as one sketch using connected lines using this command

sketch_lines = theSketch.sketchCurves.sketchLines.addByTwoPoints(theSketchLine.endSketchPoint, linePoints[iPt])

It was working perfectly fine.

Now the issue is that, in this same sketch there are small lines creating curves, so I planned to re-create the curve by using three points Arc command as seen below

arcStartPoint = theSketchLine.endSketchPoint arcEndPoint = linePoints[iPt] areJoiningPoint = linePoints[iPt-1] sketch_curves = theSketch.sketchCurves.sketchArcs.addByThreePoints(arcStartPoint, areJoiningPoint, arcEndPoint)

The issue is that the arcStartPoint is correct where it start at the endSketchpoint of the line, while the next line doesn't actually start at the end of the sketchpoint of the arc !

I think whats causing the issue is that sketchArcs and sketchLines are different skitches and they are not syncronized ? I don't know, Any ideas ?

Re: Sketching on one sketch for sweeping feature

kandennti — Mon, 06 Sep 2021 00:41:09 GMT

Hi @Anonymous .

I'm not sure what you are trying to do.

For now, I created a test code like this, but I could not find anything wrong with addByThreePoints.

# Fusion360API Python script import traceback import adsk.fusion import adsk.core def run(context): ui: adsk.core.UserInterface = None try: app: adsk.core.Application = adsk.core.Application.get() ui = app.userInterface msg: str = 'Select Sketch Curve' selFiltter: str = 'SketchCurves' sel: adsk.core.Selection = selectEnt(msg, selFiltter) if not sel: return # get points crv: adsk.fusion.SketchCurve = sel.entity pnts = getPoints(crv, 0.1) # lines createLines(pnts) # arcs createArcs(pnts) except: if ui: ui.messageBox('Failed:\n{}'.format(traceback.format_exc())) def createArcs( pnts: list): app: adsk.core.Application = adsk.core.Application.get() des: adsk.fusion.Design = app.activeProduct root: adsk.fusion.Component = des.rootComponent skt: adsk.fusion.Sketch = root.sketches.add(root.xYConstructionPlane) skt.name = 'Arcs' sktPnts = createPoints(pnts, skt) startPoints = sktPnts[0::2] joiningPoints = [p.geometry for p in sktPnts[1::2]] endPoints = sktPnts[2::2] for p1, p2, p3 in zip(startPoints, joiningPoints, endPoints): skt.sketchCurves.sketchArcs.addByThreePoints(p1, p2, p3) def createLines( pnts: list): app: adsk.core.Application = adsk.core.Application.get() des: adsk.fusion.Design = app.activeProduct root: adsk.fusion.Component = des.rootComponent skt: adsk.fusion.Sketch = root.sketches.add(root.xYConstructionPlane) skt.name = 'Lines' sktPnts = createPoints(pnts, skt) startPoints = sktPnts[0::2] endPoints = sktPnts[2::2] for p1, p2 in zip(startPoints, endPoints): skt.sketchCurves.sketchLines.addByTwoPoints(p1, p2) def createPoints( pnts: list, skt: adsk.fusion.Sketch) -> list: sktPnts = [skt.sketchPoints.add(p) for p in pnts] return sktPnts def getPoints( crv: adsk.fusion.SketchEntity, tolerance: float = 0.01) -> list: eva: adsk.core.CurveEvaluator3D = crv.worldGeometry.evaluator _, startParameter, endParameter = eva.getParameterExtents() _, vertexCoordinates = eva.getStrokes(startParameter, endParameter, tolerance) pnts = [v for v in vertexCoordinates] return pnts def selectEnt( msg: str, filtterStr: str) -> adsk.core.Selection: try: app = adsk.core.Application.get() ui = app.userInterface sel = ui.selectEntity(msg, filtterStr) return sel except: return None

Re: Sketching on one sketch for sweeping feature

Anonymous — Mon, 06 Sep 2021 03:44:28 GMT

I ran the script you provided but nothing happend !

What I wanted to do is to sketch one full path that consists of both lines and arcs.

For example Imagine I want to draw a staright line then connect to it an arc then the end point of the arc has another straight line.

What I'm getting is that the second line is starting from the end of the first line and not the end of the arc. Eventhough I'm using the command of endSketchPoint in order to keep the sketch as one full path and not segments.

The following example shows only lines connected to each other Solved: Python script to create a chain of lines - Autodesk Community - Fusion 360

Re: Sketching on one sketch for sweeping feature

kandennti — Mon, 06 Sep 2021 06:24:37 GMT

@Anonymous .

I'd love to help, but I can't reproduce the situation with only partial code.

Sketching on one sketch for sweeping feature

BrianEkins — Tue, 07 Sep 2021 13:53:24 GMT

Arcs behave differently than lines. Once an arc is created, it ALWAYS exists in a counterclockwise direction. This can mean that you can create the arc specifying the start and end points but when you query the existing arc, the start and end point may be different.

In the example below, I can create the arc by three points using points 1, 2, 3, or 3, 2, 1. However, when I query the arc to get the start and end sketch points, the start point will be 1 and the end will be point 3 because it is counterclockwise.