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Hello everyone,
my goal is to make a twisted sweep feature guided by path with known height (ex. 30.0 / 4.5) and later, merge this sweep with a cyllinder with the same height. It's important for get a smooth top surface (one planar BRepFace). All of this I can perform by API but I noticed that for some cases, especially for irrational numbers, I cannot get such surface because of difference in heights - left body:
Here's my code used for the test:
import adsk.core, adsk.fusion, traceback
import math
def createPath(sketches: adsk.fusion.Sketches,
plane: adsk.fusion.ConstructionPlane,
coordinates: adsk.core.Point2D,
height: float) -> adsk.fusion.Path:
pathSketch = sketches.add(plane)
pathSketch.name = "Path"
pathSketch.isVisible = False
line = pathSketch.sketchCurves.sketchLines.addByTwoPoints(adsk.core.Point3D.create(coordinates.x, coordinates.y, 0), adsk.core.Point3D.create(coordinates.x, coordinates.y, height))
path = plane.component.features.createPath(line)
return path
def createSweep(profile: adsk.fusion.Profile,
path: adsk.fusion.Path,
guide: adsk.fusion.Path = None,
twistAngle: float = 0) -> adsk.fusion.SweepFeature:
sweeps = profile.parentSketch.parentComponent.features.sweepFeatures
sweepInput = sweeps.createInput(profile, path, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
if guide:
sweepInput.guideRail = guide
sweepInput.profileScaling = adsk.fusion.SweepProfileScalingOptions.SweepProfileNoScalingOption
sweepInput.twistAngle = adsk.core.ValueInput.createByReal(twistAngle)
sweep = sweeps.add(sweepInput)
return sweep
def extrudeProfile(profile: adsk.fusion.Profile,
distance: float,
featureOperation: adsk.fusion.FeatureOperations = adsk.fusion.FeatureOperations.NewBodyFeatureOperation) -> adsk.fusion.ExtrudeFeature:
distanceInput = adsk.core.ValueInput.createByReal(distance)
extrusionResult = profile.parentSketch.parentComponent.features.extrudeFeatures.addSimple(profile, distanceInput, featureOperation)
return extrusionResult
def run(context):
ui = None
try:
app = adsk.core.Application.get()
ui = app.userInterface
app.documents.add(adsk.core.DocumentTypes.FusionDesignDocumentType)
product = app.activeProduct
design = adsk.fusion.Design.cast(product)
rootComp = design.rootComponent
# 1. First test - thickness as a periodic irrational number - top faces no coincident
# Prepare profile for twisting
cuboidBaseCenter = adsk.core.Point3D.create(0, 2, 0)
cuboidBaseCorner = adsk.core.Point3D.create(-0.5, 3, 0)
sketches = rootComp.sketches
twistedCuboidSketch = sketches.add(rootComp.xYConstructionPlane)
twistedCuboidSketch.name = "Twisted cuboid sketch 1"
twistedCuboidSketch.isVisible = False
twistedCuboidSketch.sketchCurves.sketchLines.addCenterPointRectangle(cuboidBaseCenter, cuboidBaseCorner)
# Prepare profile for core
coreRadius = 1.3
coreCenter = rootComp.originConstructionPoint.geometry
coreSketch = sketches.add(rootComp.xYConstructionPlane)
coreSketch.name = "Core sketch 1"
coreSketch.isVisible = False
coreSketch.sketchCurves.sketchCircles.addByCenterRadius(coreCenter, coreRadius)
# Create twisted cuboid
thickness = 30.0 / 4.5
path = createPath(sketches, rootComp.xYConstructionPlane, adsk.core.Point2D.create(0, 0), thickness)
createSweep(twistedCuboidSketch.profiles.item(0), path, twistAngle=math.pi / 2)
# Merge it with core
extrudeProfile(coreSketch.profiles.item(0), thickness, adsk.fusion.FeatureOperations.JoinFeatureOperation)
# 2. Second test - thickness as a finite number - top faces coincident
# Prepare profile for twisting
cuboidBaseCenter = adsk.core.Point3D.create(10, 2, 0)
cuboidBaseCorner = adsk.core.Point3D.create(9.5, 3, 0)
sketches = rootComp.sketches
twistedCuboidSketch = sketches.add(rootComp.xYConstructionPlane)
twistedCuboidSketch.name = "Twisted cuboid sketch 2"
twistedCuboidSketch.isVisible = False
twistedCuboidSketch.sketchCurves.sketchLines.addCenterPointRectangle(cuboidBaseCenter, cuboidBaseCorner)
# Prepare profile for core
coreRadius = 1.3
coreCenter = adsk.core.Point3D.create(10, 0, 0)
coreSketch = sketches.add(rootComp.xYConstructionPlane)
coreSketch.name = "Core sketch 2"
coreSketch.isVisible = False
coreSketch.sketchCurves.sketchCircles.addByCenterRadius(coreCenter, coreRadius)
# Create twisted cuboid
thickness = 30.0 / 1.5
path = createPath(sketches, rootComp.xYConstructionPlane, adsk.core.Point2D.create(10, 0), thickness)
createSweep(twistedCuboidSketch.profiles.item(0), path, twistAngle=math.pi / 2)
# Merge it with core
extrudeProfile(coreSketch.profiles.item(0), thickness, adsk.fusion.FeatureOperations.JoinFeatureOperation)
except:
if ui:
ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))I also tried:
- extrude circle to top twisted body (as isMinSolution = False) but I got error because circle profile is outside of the top face,
- make a plane on top face of twisted body (offset zero) and extrude the circle to this plane but it caused error which closed the Fusion,
- get a point from the top face (face.pointOnFace) and extrude the circle to facePoint.z but it doesn't help - result the same.
Of course, if hight is a fraction I can prepare higher (height as int number) body with apropriate modified angle and later cut this body for desired size, but is there a better solution?
Thank you
I thought about using a plane, but I tried using a formula.
Perhaps I thought that the data would be cleaner.
Attach the sprict file.
It was also a study for me.
The reason is that "30.0 / 4.5" is an Irrational number (Circulating decimal).
Added to the first code.
・・・
# Merge it with core
extrude = extrudeProfile(coreSketch.profiles.item(0), thickness, adsk.fusion.FeatureOperations.JoinFeatureOperation)
#path length
pathLine = adsk.fusion.SketchLine.cast(path.item(0).entity)
geoSt = pathLine.startSketchPoint.geometry
geoEd = pathLine.endSketchPoint.geometry
pathLengthResult = geoSt.distanceTo(geoEd)
#extrude distance
extrudeDistanceResult = extrude.extentOne.distance.value
ui.messageBox('pathLength:{}\nextrudeDistance:{}'
.format(pathLengthResult,extrudeDistanceResult))
# 2. Second test - thickness as a finite number - top faces coincident
・・・
The result is as follows.
Until using the API, it may be better to use mathematical formulas.
I was interested, so I tried a little more.
Even without using an formula, just assigning the value to the value of modelParameter again gave the correct result.
Just modify the extrudeProfile function in the first code and you will get the correct result.
・・・
def extrudeProfile(profile: adsk.fusion.Profile,
distance: float,
featureOperation: adsk.fusion.FeatureOperations = adsk.fusion.FeatureOperations.NewBodyFeatureOperation) -> adsk.fusion.ExtrudeFeature:
distanceInput = adsk.core.ValueInput.createByReal(distance)
extrusionResult = profile.parentSketch.parentComponent.features.extrudeFeatures.addSimple(profile, distanceInput, featureOperation)
#Enter an value in modelParam
distParamName = extrusionResult.extentOne.distance.name
modelParams = extrusionResult.parentComponent.parentDesign.rootComponent.modelParameters
param = modelParams.itemByName(distParamName)
param.value = distance
return extrusionResult
・・・
I thought "ValueInput.createByReal" might be the cause and created the following test code.
import adsk.core
def run(context):
app = adsk.core.Application.get()
ui = app.userInterface
float_Value = 30.0/4.5
ValueInputReal = adsk.core.ValueInput.createByReal(float_Value)
ui.messageBox('float_Value : {}\nValueInputReal : {}'
.format(float_Value,ValueInputReal.realValue))
This is not the cause....
I was also interested and finally found the cause. In case of every feature which need "valueInput" for entering dimensions/angles the value in such input is automatically rounded according to general precision (definded in "preferences" window):
I think in the second case error is bigger than tollerance and merging bodies doesn't treat those two BRepFace as one.
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