# Author - Nadieh Bremer # Description - Create a ceiling light construction that rotates from one end to the other import math import adsk.core import adsk.fusion # import adsk.cam import traceback # Remap a value from a range of [in_min, in_max] to [out_min, out_max] def remap(x, in_min, in_max, out_min, out_max): return (x - in_min) * (out_max - out_min) / (in_max - in_min) + out_min # Easing function # Modeled after the parabola y = -x^2 + 2x # https://gist.github.com/zeffii/c1e14dd6620ad855d81ec2e89a859719 def QuadraticEaseOut(p, start=0, end=1): norm = p/end value = -(norm * (norm - 2)) remappedValue = remap(value, 0, 1, start, end) return remappedValue # Create the points for the slices and all the slots def createDoubleCurves(j, steps, loops, radius, thickness, millRadius, a, sliceDistance, radiusFactor, offsetFactor, slotDepth, paramMaterialThickness, sign): # Create an object collection for the points. points = adsk.core.ObjectCollection.create() ribPoint = 0 jointPositions = [0, 0] jointPositionsRib = [0, 0] centerPointsCircles = [0, 0] centerPointsCirclesRib = [0, 0] for i in range(steps): # from 0 to TWOPI radians p = (i / steps) * math.pi * 2 slicePosition = (j+1) * sliceDistance offset = math.cos((i % loops) / loops * math.pi * 2 + a * loops) * 1.35 offset = offset * radiusFactor # From circle to hexagon and back offset = offset * offsetFactor # Inside or outside curve if sign == 1: offset = offset * (9 + thickness)/9 # 1.16 else: offset = offset * (9 - thickness)/9 # 0.84 x = (radius + offset + sign * thickness) * math.cos(p) y = (radius + offset + sign * thickness) * math.sin(p) points.add(adsk.core.Point3D.create(x, y, slicePosition)) # Points for rectangle to create slots if i == 0: jointPositions = [adsk.core.Point3D.create(x, y, slicePosition), adsk.core.Point3D.create(x + slotDepth, y + paramMaterialThickness / 2, slicePosition)] # Points for rectangle to create slots jointPositionsRib = [adsk.core.Point3D.create(slicePosition, x + 2*slotDepth, y), adsk.core.Point3D.create(slicePosition + paramMaterialThickness / 2, x + slotDepth, y)] # Points for t-bone circle if i == 0: centerPointsCircles = [adsk.core.Point3D.create(x + slotDepth - millRadius, y + paramMaterialThickness / 2, slicePosition), adsk.core.Point3D.create(x + slotDepth - millRadius, y - paramMaterialThickness / 2, slicePosition)] # Points for rectangle to create slots centerPointsCirclesRib = [adsk.core.Point3D.create(slicePosition + paramMaterialThickness / 2, x + slotDepth + millRadius, y), adsk.core.Point3D.create(slicePosition - paramMaterialThickness / 2, x + slotDepth + millRadius, y)] # Create rib point if i == 0: position = 0 if sign == 1: position = -1 else: position = 2 x = (radius + offset + sign * (thickness + position)) * math.cos(p) y = (radius + offset + sign * (thickness + position)) * math.sin(p) ribPoint = adsk.core.Point3D.create(slicePosition, x, y) # Add the first point to create a closed loop points.add(points.item(0)) return points, ribPoint, jointPositions, jointPositionsRib, centerPointsCircles, centerPointsCirclesRib 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. rootComp = design.rootComponent # Create a new sketch on the xy plane. sketches = rootComp.sketches yzPlane = rootComp.yZConstructionPlane xzPlane = rootComp.xZConstructionPlane sketch = sketches.add(yzPlane) sketchRib = sketches.add(xzPlane) # Get extrude features extrudes = rootComp.features.extrudeFeatures # Creating fillets fillets = rootComp.features.filletFeatures # Create slot rectangle inside the ribs lines = sketch.sketchCurves.sketchLines linesRib = sketchRib.sketchCurves.sketchLines # Create t-bone circle circles = sketch.sketchCurves.sketchCircles circlesRib = sketchRib.sketchCurves.sketchCircles # Get the user parameters userParams = design.userParameters paramMaterialThickness = userParams.itemByName('material_thickness').value paramRingThickness = userParams.itemByName('ring_thickness').value # Important Constants radiusBase = 9 thickness = paramRingThickness/2 slotDepth = 1.5 millRadius = 0.5/2 #5mm loops = 6 # How many points to sample along a sine curve steps = 6 * loops # How many points along a circle are created for each slice sliceDistance = 3 # The distance between each slice curveItems = 49 #math.round(150/sliceDistance) # The number of slices, uneven ####################################################### # Create Curved Slices ####################################################### ribPointsInside = adsk.core.ObjectCollection.create() ribPointsOutside = adsk.core.ObjectCollection.create() ribPointsSlots = adsk.core.ObjectCollection.create() ribCirclePoints = adsk.core.ObjectCollection.create() # Define the points the spline with fit through for j in range(-1, curveItems - 1, 1): # Get an adjusted index that runs from 0 to half the number of slices with an easing function index = j if j > math.floor((curveItems - 1 - 1) / 2): index = curveItems - 1 - 1 - 1 - j index = QuadraticEaseOut(index, start=0, end=math.floor((curveItems - 2) / 2)) # Get the radius that slowly increases and decreases again radiusFactor = remap(index, 0, math.floor((curveItems - 2) / 2), 0.5, 1.0) radius = radiusBase * radiusFactor # Let it go from a circle to the full shape and back offsetFactor = remap(index, 0, math.floor((curveItems - 2) / 2), 0, 1) # Slowly rotate each slice a = j / (curveItems-3) * math.pi # Create the inner curve pointsInside = createDoubleCurves(j, steps, loops, radius, thickness, millRadius, a, sliceDistance, radiusFactor, offsetFactor, slotDepth, paramMaterialThickness, -1) # Create the outer curve pointsOutside = createDoubleCurves(j, steps, loops, radius, thickness, millRadius, a, sliceDistance, radiusFactor, offsetFactor, slotDepth, paramMaterialThickness, 1) # Don't actually add the first and last curve if j > -1 and j < curveItems - 2: # Create a spline along those points spline = sketch.sketchCurves.sketchFittedSplines.add(pointsInside[0]) spline.isClosed = True # Create a spline along those points spline = sketch.sketchCurves.sketchFittedSplines.add(pointsOutside[0]) spline.isClosed = True # Create slot rectangle lines.addCenterPointRectangle(pointsInside[2][0], pointsInside[2][1]) # Create circles for t-bones circles.addByCenterRadius(pointsInside[4][0], millRadius) circles.addByCenterRadius(pointsInside[4][1], millRadius) # Add the rectangles for the ribs ribPointsSlots.add(pointsInside[3][0]) ribPointsSlots.add(pointsInside[3][1]) # Add the circles for the t-bones for the ribs ribCirclePoints.add(pointsInside[5][0]) ribCirclePoints.add(pointsInside[5][1]) # Add the first item of each outer spline to a "rib" ribPointsInside.add(pointsInside[1]) ribPointsOutside.add(pointsOutside[1]) ####################################################### # Extrude Section Between Curves ####################################################### # https://forums.autodesk.com/t5/fusion-360-api-and-scripts/extruding-multiple-profiles-from-one-sketch/td-p/6026535 # Create an object collection to use an input # To be able to extrude all profiles in one go profs = adsk.core.ObjectCollection.create() # Get the profiles # profs.add(sketch.profiles.item(8)) for j in range(curveItems-2): profs.add(sketch.profiles.item(j*8)) # when using offsets - including t-bones # profs.add(sketch.profiles.item(j*4)) # when using offsets - no t-bones # Define a distance extent extrudeDistance = adsk.core.ValueInput.createByString("material_thickness") # Create the extrusion extrudeInput = extrudes.createInput(profs, adsk.fusion.FeatureOperations.NewBodyFeatureOperation) extrudeInput.setSymmetricExtent(extrudeDistance, True) extrudeSlices = extrudes.add(extrudeInput) # ####################################################### # # Fillet the Slots # ####################################################### # #Create a collection to hold the edges # edgeCollection = adsk.core.ObjectCollection.create() # # # body = extrudeResult.bodies.item(0) # # #Loop over all the bodies in the extrusion result # for body in extrudeSlices.bodies: # edgeCollection.add(body.edges.item(7)) # edgeCollection.add(body.edges.item(9)) # #14 items per body # # # https://forums.autodesk.com/t5/fusion-360-api-and-scripts/extruding-profile-collection-in-single-operation/td-p/7905790 # # https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-7105bf44-52db-4067-8d7a-afd73c24e954 # filletRadius = adsk.core.ValueInput.createByReal((.25)) # filletInput = fillets.createInput() # filletInput.addConstantRadiusEdgeSet(edgeCollection, filletRadius, True) # filletInput.isG2 = False # filletInput.isRollingBallCorner = True # fillet = fillets.add(filletInput) ####################################################### # Create Rib Spline ####################################################### # Add the outside rib to the inner side, but in reverse order for j in reversed(range(curveItems)): ribPointsInside.add(ribPointsOutside.item(j)) # Turn into a spline spline = sketchRib.sketchCurves.sketchFittedSplines.add(ribPointsInside) spline.isClosed = True for j in range(curveItems - 2): linesRib.addCenterPointRectangle(ribPointsSlots.item(j*2), ribPointsSlots.item(j*2 + 1)) circlesRib.addByCenterRadius(ribCirclePoints.item(j*2), millRadius) circlesRib.addByCenterRadius(ribCirclePoints.item(j*2 + 1), millRadius) # Get the profile of the rib spline profs = adsk.core.ObjectCollection.create() # To test: # for j in range(0, 30, 1): # profs.add(sketchRib.profiles.item(j)) # Either the 0th profile or something late in the line # Total number = (curveItems-2) * 6 + 1? - for t-bones profs.add(sketchRib.profiles.item(6*(curveItems-2) - 0)) # profs = sketchRib.profiles.item(2*(curveItems-2) - 1) # number 103 for 54 slices, 105 profiles - no t-bones # profs = sketchRib.profiles.item(11) #number 11 for 8 slices, 13 profiles max - no t-bones extrudeDistance = adsk.core.ValueInput.createByString("material_thickness") # Extrude the rib, symmetrically extrudeInput = extrudes.createInput(profs, adsk.fusion.FeatureOperations.NewBodyFeatureOperation) extrudeInput.setSymmetricExtent(extrudeDistance, True) extrudeRib = extrudes.add(extrudeInput) # ####################################################### # # Fillet the Rib Slots # ####################################################### # # # Create a collection to hold the edges # edgeCollection = adsk.core.ObjectCollection.create() # # # Add very specific edges # body = extrudeRib.bodies.item(0) # start = 2 + (curveItems-2)*4 # for j in range(curveItems-2): # edgeCollection.add(body.edges.item(start+1 + j*8)) # edgeCollection.add(body.edges.item(start+7 + j*8)) # # edgeCollection.add(body.edges.item(start+1)) # # filletRadius = adsk.core.ValueInput.createByReal((.125)) # filletInput = fillets.createInput() # filletInput.addConstantRadiusEdgeSet(edgeCollection, filletRadius, True) # filletInput.isG2 = False # filletInput.isRollingBallCorner = True # fillet = fillets.add(filletInput) except: if ui: ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))