Hi @2way3dtext .
I only saw "Error Script revolve both ends".
The easiest solution was to get the profile just before doing revolves.createInput.
・・・
profile_2 = sketch_2.profiles.item(0)
profile_1 = sketch_1.profiles.item(0) # <-Here
# Create an revolution input to be able to define the input needed for a revolution
# while specifying the profile and that a new component is to be created
revolves = comp.features.revolveFeatures
revInput_1 = revolves.createInput(
profile_1, axisLine_1, adsk.fusion.FeatureOperations.NewComponentFeatureOperation)
revInput_2 = revolves.createInput(
profile_2, axisLine_2, adsk.fusion.FeatureOperations.NewComponentFeatureOperation)
・・・
I don't know the exact cause of the error, but I think it's because I'm creating Dimensions and Constraints after getting the profile.
I think if you get what you need when you need it, you can avoid the error.
(There are so many variables in one function that I can't keep track of them all in my head.)
If I were to Refactoring this, it would be the creation of two sketches that would be needed as profiles.
If I were to refactoring this, I would create two sketches that I would need as profiles, and since the two sketches are almost identical, I would consider having them processed by a single function.
import adsk.core
import adsk.fusion
import adsk.cam
import traceback
import math
def run(context):
ui = None
try:
app = adsk.core.Application.get()
ui = app.userInterface
design = app.activeProduct
unitsMgr = design.fusionUnitsManager
unitsMgr.distanceDisplayUnits = adsk.fusion.DistanceUnits.MillimeterDistanceUnits
# pipe diameter
pipeDiameter = 1
pipeRadius = pipeDiameter * 0.5
# select edge
sel = ui.selectEntity(
'Select a path to create a pipe', 'Edges,SketchCurves')
selObj = sel.entity
comp = design.rootComponent
# create path
feats = comp.features
chainedOption = adsk.fusion.ChainedCurveOptions.noChainedCurves
path = adsk.fusion.Path.create(selObj, chainedOption)
# get construction Planes
planes = comp.constructionPlanes
# create construction plane_1
planeInput = planes.createInput()
planeInput.setByDistanceOnPath(
selObj, adsk.core.ValueInput.createByReal(0))
plane_1 = planes.add(planeInput)
# create construction plane_2
planeInput.setByDistanceOnPath(
selObj, adsk.core.ValueInput.createByReal(1))
plane_2 = planes.add(planeInput)
# create Profile Sketch
sketch_1: adsk.fusion.Sketch = createProfileSketch(plane_1, pipeRadius)
sketch_2: adsk.fusion.Sketch = createProfileSketch(plane_2, pipeRadius)
# Create an revolution input to be able to define the input needed for a revolution
# while specifying the profile and that a new component is to be created
revolves = comp.features.revolveFeatures
revInput_1 = revolves.createInput(
sketch_1.profiles[0],
sketch_1.sketchCurves.sketchLines[0],
adsk.fusion.FeatureOperations.NewBodyFeatureOperation
)
revInput_2 = revolves.createInput(
sketch_2.profiles[0],
sketch_2.sketchCurves.sketchLines[0],
adsk.fusion.FeatureOperations.NewBodyFeatureOperation
)
# Define that the extent is an angle of 2*pi to get a sphere
angle = adsk.core.ValueInput.createByReal(2*math.pi)
revInput_1.setAngleExtent(False, angle)
revInput_2.setAngleExtent(False, angle)
# Create the extrusion.
ext_1 = revolves.add(revInput_1)
ext_2 = revolves.add(revInput_2)
# Create an object collection to use an input.
profs = adsk.core.ObjectCollection.create()
# Add all of the profiles to the collection.
for prof in sketch_2.profiles:
profs.add(prof)
# create sweep
sweepFeats = feats.sweepFeatures
sweepInput = sweepFeats.createInput(
profs, path, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
sweepInput.orientation = adsk.fusion.SweepOrientationTypes.PerpendicularOrientationType
sweepFeat = sweepFeats.add(sweepInput)
except:
if ui:
ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
def createProfileSketch(
refPlane: adsk.fusion.ConstructionPlane,
pipeRadius: float) -> adsk.fusion.Sketch:
# get sketches
sketches: adsk.fusion.Sketches = refPlane.component.sketches
# create sketch
sketch: adsk.fusion.Sketch = sketches.add(refPlane)
# circle
circles: adsk.fusion.SketchCircle = sketch.sketchCurves.sketchCircles
circle: adsk.fusion.SketchCircle = circles.addByCenterRadius(
adsk.core.Point3D.create(0, 0, 0), pipeRadius)
# axis line
lines: adsk.fusion.SketchLines = sketch.sketchCurves.sketchLines
axisLine: adsk.fusion.SketchLine = lines.addByTwoPoints(
adsk.core.Point3D.create(-pipeRadius, 0, 0),
adsk.core.Point3D.create(pipeRadius, 0, 0)
)
# dimension
dimensions: adsk.fusion.SketchDimensions = sketch.sketchDimensions
dimensions.addDistanceDimension(
axisLine.startSketchPoint,
axisLine.endSketchPoint,
adsk.fusion.DimensionOrientations.AlignedDimensionOrientation,
circle.centerSketchPoint.geometry
)
textPoint: adsk.core.Point3D = circle.centerSketchPoint.geometry
textPoint.translateBy(
adsk.core.Vector3D.create(0.001, 0.001, 0.001)
)
dimensions.addRadialDimension(circle, textPoint)
# geometricConstraints
constraints: adsk.fusion.GeometricConstraints = sketch.geometricConstraints
constraints.addCoincident(
axisLine.startSketchPoint,
circle
)
constraints.addCoincident(
axisLine.endSketchPoint,
circle
)
constraints.addHorizontal(axisLine)
setDimension(circle)
return sketch
def setDimension(
self: adsk.fusion.SketchCircle):
skt: adsk.fusion.Sketch = self.parentSketch
ori: adsk.fusion.SketchPoint = skt.sketchPoints.item(0)
ctr: adsk.fusion.SketchPoint = self.centerSketchPoint
ary = [(o + c) * 0.5 for (o, c) in
zip(ori.geometry.asArray(), ctr.geometry.asArray())]
mid: adsk.core.Point3D = ori.geometry.copy()
mid.setWithArray(ary)
dims: adsk.fusion.SketchDimensions = skt.sketchDimensions
h = adsk.fusion.DimensionOrientations.HorizontalDimensionOrientation
v = adsk.fusion.DimensionOrientations.VerticalDimensionOrientation
dims.addDistanceDimension(ori, ctr, h, mid, True)
dims.addDistanceDimension(ori, ctr, v, mid, True)
This is still not enough.
