topic Betreff: How can I use an edge as a profile for a not solid sweep (surface)? in Fusion API and Scripts Forum

How can I use an edge as a profile for a not solid sweep (surface)?

adminTCYL2 — Mon, 13 Sep 2021 18:34:36 GMT

I use rotated sweeps as basis to draw electrical coils. This works best on lines or arcs and not good on splines.

The basis curve is done by a formular. So I get points and normaly I would draw a spline along, but in this case it is better to draw arcs along. Then I do this rotated sweeps along the arcs.

But there is a problem: Each surface has its own profile and they do not connect.
To connect them to one surface I want to use the end-edge of an arc-sweep as profile for the next arc-sweep.

In my script you see out comanded lines where I try this. But Fusion does not accept the edge as a profile.
Does someone know a solution?

import adsk.core, adsk.fusion, adsk.cam, traceback, math def run(context): ui = None try: app = adsk.core.Application.get() ui = app.userInterface design = app.activeProduct # Get the root component of the active design. root_comp = design.rootComponent # Create a new sketch on the xy plane. sketches = root_comp.sketches xyPlane = root_comp.xYConstructionPlane sketch = sketches.add(xyPlane) points = adsk.core.ObjectCollection.create() # Create an object collection for the points. windings = 10 pointsPerRound = 4 # Number of points that splines are generated. i = -pointsPerRound*windings #Startwert, der in der Schleife runtergezählt wird r = 0.5 h = 0 while i <= 0: t = (math.pi/(pointsPerRound*windings))*i*2 h = 1.5+((-r)*(math.sin(t*windings))) xCoord = (h)*(math.sin(t)) yCoord = (h)*(math.cos(t)) zCoord = ((-r)*(math.cos(t*windings))) points.add(adsk.core.Point3D.create(xCoord,yCoord,zCoord)) i = i + 1 #Combining the points to arcs arcs = adsk.core.ObjectCollection.create() for j in range(0,int((windings*pointsPerRound)/2)): arc = sketch.sketchCurves.sketchArcs.addByThreePoints(points[2*j],points[2*j+1],points[2*j+2]) arcs.add(arc) profilStart = adsk.core.Point3D.create(points[2*j].x,points[2*j].y,points[2*j].z-0.2) profilEnd = adsk.core.Point3D.create(points[2*j].x,points[2*j].y,points[2*j].z-0.01) profil=sketch.sketchCurves.sketchLines.addByTwoPoints(profilStart,profilEnd) """ # The right way would be: define a start profile for the sweep... if j==0: profilStart = adsk.core.Point3D.create(points[0].x,points[0].y,points[0].z-0.2) profilEnd = adsk.core.Point3D.create(points[0].x,points[0].y,points[0].z-0.01) profil=sketch.sketchCurves.sketchLines.addByTwoPoints(profilStart,profilEnd) # ..and then use the edge of the last sweep as profile for the next: else: itemIndex = root_comp.bRepBodies.count-1 body = root_comp.bRepBodies.item(itemIndex) profil= body.edges.item(3) #it is not clear witch of the four items sketch.add(profil) """ prof = root_comp.createOpenProfile(profil, False) path = root_comp.features.createPath(arc, False) sweeps = root_comp.features.sweepFeatures sweepInput1 = sweeps.createInput(prof, path, adsk.fusion.FeatureOperations.NewBodyFeatureOperation) sweepInput1.twistAngle = adsk.core.ValueInput.createByReal(100) sweepInput1.isSolid = False sweep = sweeps.add(sweepInput1) for j in range(0,10): arcs[j].startSketchPoint.merge(arcs[j+1].endSketchPoint) except: if ui: ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

Re: How can I use an edge as a profile for a not solid sweep (surface)?

kandennti — Tue, 14 Sep 2021 07:07:08 GMT

Hi @adminTCYL2 .

It looked interesting, so I gave it a try.

I decided to create only one SketchLine, which would be the profile of the first Sweep, and use the edge of the previous Sweep for the rest of the Sweeps.

# Fusion360API Python script import adsk.core, adsk.fusion, traceback, math def run(context): ui = None try: app = adsk.core.Application.get() ui = app.userInterface design = app.activeProduct # Get the root component of the active design. root_comp = design.rootComponent windings = 10 pointsPerRound = 4 # Number of points that splines are generated. i = -pointsPerRound*windings #Startwert, der in der Schleife runtergezählt wird r = 0.5 h = 0 # create points points = [] while i <= 0: t = (math.pi/(pointsPerRound*windings))*i*2 h = 1.5+((-r)*(math.sin(t*windings))) xCoord = (h)*(math.sin(t)) yCoord = (h)*(math.cos(t)) zCoord = ((-r)*(math.cos(t*windings))) points.append( adsk.core.Point3D.create(xCoord,yCoord,zCoord) ) i = i + 1 # create sketch sketches = root_comp.sketches xyPlane = root_comp.xYConstructionPlane sketch: adsk.fusion.Sketch = sketches.add(xyPlane) sketch.arePointsShown = False # create arcs sketch.isComputeDeferred = True sktArcs = sketch.sketchCurves.sketchArcs arcs = [sktArcs.addByThreePoints(p1, p2, p3) for p1, p2, p3 in zip(points[0::2], points[1::2], points[2::2])] # create start line & OpenProfile line: adsk.fusion.SketchLine = sketch.sketchCurves.sketchLines.addByTwoPoints( adsk.core.Point3D.create( points[0].x, points[0].y, points[0].z - 0.2 ), adsk.core.Point3D.create( points[0].x, points[0].y, points[0].z - 0.01 ) ) profile: adsk.fusion.Profile = root_comp.createOpenProfile(line) sketch.isComputeDeferred = False # create paths paths = [root_comp.features.createPath(arc, False) for arc in arcs] # create SweepFeatureInput - This is only temporary. sweeps: adsk.fusion.SweepFeatures = root_comp.features.sweepFeatures twistAngle = adsk.core.ValueInput.createByReal(100) sweepIpt: adsk.fusion.SweepFeatureInput = sweeps.createInput( profile, paths[0], adsk.fusion.FeatureOperations.NewBodyFeatureOperation ) sweepIpt.isSolid = False sweepIpt.twistAngle = twistAngle # create SweepFeature # Create a SweepFeature while modifying SweepFeatureInput. # Find the edge that will be the next profile from the SweepFeature. for path in paths: sweepIpt.profile = profile sweepIpt.path = path sweepFeat: adsk.fusion.SweepFeature = sweeps.add(sweepIpt) edge: adsk.fusion.BRepEdge = findNextProfileEdge(sweepFeat) profile = root_comp.createBRepEdgeProfile(edge, False) except: if ui: ui.messageBox('Failed:\n{}'.format(traceback.format_exc())) def findNextProfileEdge( sweepFeat: adsk.fusion.SweepFeature) -> adsk.fusion.BRepEdge: profileGeo: adsk.core.Line3D = sweepFeat.profile.item(0).entity.geometry nextProfileEdge = None edge: adsk.fusion.BRepEdge for edge in sweepFeat.sideFaces[0].edges: if edge.geometry.objectType != 'adsk::core::Line3D': continue if not idEqualLine(profileGeo, edge.geometry): nextProfileEdge = edge break if not nextProfileEdge: raise ValueError("Cannot find the next profile!") return nextProfileEdge def idEqualLine( l1: adsk.core.Line3D, l2: adsk.core.Line3D) -> bool: if not l1.isColinearTo(l2): return False p1: adsk.core.Point3D = l2.startPoint p2: adsk.core.Point3D = l2.endPoint if l1.startPoint.isEqualTo(p1): if l1.endPoint.isEqualTo(p2): return True elif l1.startPoint.isEqualTo(p2): if l1.endPoint.isEqualTo(p1): return True return False

I don't know about these shapes, but since the Arcs are not smoothly connected, the resulting Surface is not smooth either.

Also, the first and last edges were not connected.
I think it was a problem with the twist angle calculation, but I couldn't figure out what was right.

Re: How can I use an edge as a profile for a not solid sweep (surface)?

kandennti — Tue, 14 Sep 2021 07:29:54 GMT

@adminTCYL2 .

I forgot to write down the most important thing.
It is the Component.createBRepEdgeProfile method that gets the profile from the edge.

https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-ca25aae8-7ca2-4048-b912-e980774a736e

Betreff: How can I use an edge as a profile for a not solid sweep (surface)?

adminTCYL2 — Tue, 14 Sep 2021 08:07:22 GMT

Thank you kandennti, that is a great peace of work!
With the Component.createBRepEdgeProfile method I can now use edges as profiles by simply write:

prof = root_comp.createBRepEdgeProfile(edge, False)

But using it in my script worked just for the first three arcs. Then the body.edges.item(2) was the wrong one... somehow the item-number of the ages change by position of the surface... and so further arcs failed.
I wonder how you managed to solve this problem! I will try to understand your code and give further feedback.

Betreff: How can I use an edge as a profile for a not solid sweep (surface)?

adminTCYL2 — Tue, 14 Sep 2021 08:56:38 GMT

Hi Kandennti,
I tested your script. It works very fine. The only change I did was not to calculate all parts (arcs) and enhanced the calculated points so that the arcs are short and the coil is very near to the mathematical optimum.
As you see this script allows very many rotations and can be basis for drawing electrical coils along the edge of the sweeps. I accepted your solution, because this script is your success not mine. I would not have been able to write this nice function to choose allways the right edge.

# Fusion360API Python script import adsk.core, adsk.fusion, traceback, math def run(context): ui = None try: # Settings: windings = 10 pointsPerRound = 20 # Number of points that splines are generated. calculatedArcs = 20 # All are calculated by windings*pointsPerRound/2 r = 0.5 h = 0 rotations=100 app = adsk.core.Application.get() ui = app.userInterface design = app.activeProduct root_comp = design.rootComponent # create points points = [] i = -pointsPerRound*windings while i <= 0: t = (math.pi/(pointsPerRound*windings))*i*2 h = 1.5+((-r)*(math.sin(t*windings))) xCoord = (h)*(math.sin(t)) yCoord = (h)*(math.cos(t)) zCoord = ((-r)*(math.cos(t*windings))) points.append( adsk.core.Point3D.create(xCoord,yCoord,zCoord) ) i = i + 1 # create sketch sketches = root_comp.sketches xyPlane = root_comp.xYConstructionPlane sketch: adsk.fusion.Sketch = sketches.add(xyPlane) sketch.arePointsShown = False # create arcs sketch.isComputeDeferred = True sktArcs = sketch.sketchCurves.sketchArcs arcs = [sktArcs.addByThreePoints(p1, p2, p3) for p1, p2, p3 in zip(points[0::2], points[1::2], points[2::2])] # create start line & OpenProfile line: adsk.fusion.SketchLine = sketch.sketchCurves.sketchLines.addByTwoPoints( adsk.core.Point3D.create( points[0].x, points[0].y, points[0].z - 0.2 ), adsk.core.Point3D.create( points[0].x, points[0].y, points[0].z - 0.01 ) ) profile: adsk.fusion.Profile = root_comp.createOpenProfile(line) sketch.isComputeDeferred = False # create paths paths = [root_comp.features.createPath(arc, False) for arc in arcs] # create SweepFeatureInput - This is only temporary. sweeps: adsk.fusion.SweepFeatures = root_comp.features.sweepFeatures twistAngle = adsk.core.ValueInput.createByReal(rotations) sweepIpt: adsk.fusion.SweepFeatureInput = sweeps.createInput( profile, paths[0], adsk.fusion.FeatureOperations.NewBodyFeatureOperation ) sweepIpt.isSolid = False sweepIpt.twistAngle = twistAngle # create SweepFeature # Create a SweepFeature while modifying SweepFeatureInput. # Find the edge that will be the next profile from the SweepFeature. for j in range (0,calculatedArcs): #for path in paths: sweepIpt.profile = profile sweepIpt.path = paths[j] # =path sweepFeat: adsk.fusion.SweepFeature = sweeps.add(sweepIpt) edge: adsk.fusion.BRepEdge = findNextProfileEdge(sweepFeat) profile = root_comp.createBRepEdgeProfile(edge, False) except: if ui: ui.messageBox('Failed:\n{}'.format(traceback.format_exc())) def findNextProfileEdge( sweepFeat: adsk.fusion.SweepFeature) -> adsk.fusion.BRepEdge: profileGeo: adsk.core.Line3D = sweepFeat.profile.item(0).entity.geometry nextProfileEdge = None edge: adsk.fusion.BRepEdge for edge in sweepFeat.sideFaces[0].edges: if edge.geometry.objectType != 'adsk::core::Line3D': continue if not idEqualLine(profileGeo, edge.geometry): nextProfileEdge = edge break if not nextProfileEdge: raise ValueError("Cannot find the next profile!") return nextProfileEdge def idEqualLine( l1: adsk.core.Line3D, l2: adsk.core.Line3D) -> bool: if not l1.isColinearTo(l2): return False p1: adsk.core.Point3D = l2.startPoint p2: adsk.core.Point3D = l2.endPoint if l1.startPoint.isEqualTo(p1): if l1.endPoint.isEqualTo(p2): return True elif l1.startPoint.isEqualTo(p2): if l1.endPoint.isEqualTo(p1): return True return False