I used Inventor during my Ph.D. and now I want to port and existing piece of software to create patterns on highly curved surfaces automatically. But I can not find a couple of calls used the Inventor API inside of FUSION. One of them is the CalculateFacets() method http://adndevblog.typepad.com/manufacturing/2013/11/getexistingfacets-and-calculatefacets.html
Here some examples of what I can do using the tool on Inventor. Any suggestions on where to look first?
Thank you
The equivalent of the CalculateFacets method in Fusion is that from the BRepBody or BRepFace object you can get a MeshManager object using the meshManager property on each of those objects. The MeshManager object lets you accessing the existing display meshes but also supports the createMeshCalculator method. On the MeshCalculator object you can set various parameters to control how the mesh is calculated and then call the calculate method which returns a TriangleMesh object that has all of the information about the mesh. Below is something similar to what you've done that I did with this functionality in Fusion.
Here's the model and program that I used in the image I posted earlier. The program is fairly rough since it was just a proof of concept. There are two functions; one that creates the points on the surface and the second one positions a selected component at the point at a specified depth and random orientation and subtracts it from the model.
import adsk.core, adsk.fusion, traceback
import random, math
def run(context):
ui = None
try:
app = adsk.core.Application.get()
ui = app.userInterface
#createPoints()
createGouges()
#ui.messageBox('U: ' + str(avgULength) + ', V: ' + str(avgVLength))
except:
if ui:
ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
def createGouges():
ui = None
try:
app = adsk.core.Application.get()
ui = app.userInterface
des = app.activeProduct
root = adsk.fusion.Component.cast(des.rootComponent)
# Have the body selected.
face = ui.selectEntity('Select a face on the body to cut', 'Faces').entity
mainBody = face.body
# Have the sketch with the points selected.
sketch = ui.selectEntity('Select a sketch in the browser', 'Sketches').entity
# Have the gouge occurrence selected.
occ = ui.selectEntity('Select a component', 'Occurrences').entity
gougeBody = occ.bRepBodies.item(0)
mainBody.isVisible = False
baseFeature = root.features.baseFeatures.add()
baseFeature.startEdit()
targetBody = mainBody.copyToComponent(root)
targetBody.isVisible = True
adsk.doEvents()
pnts = []
first = True
for skPnt in sketch.sketchPoints:
if not first:
pnts.append(skPnt.geometry)
else:
first = False
surfEval = face.evaluator
(returnValue, normals) = surfEval.getNormalsAtPoints(pnts)
ui.messageBox('Number of gouges that will be created: ' + str(len(pnts)))
depth = 0.75
toolBodies = adsk.core.ObjectCollection.create()
for i in range(0, len(pnts)):
# Compute the origin of the gouge using the specified depth.
# The depth could be random but it's not implemented yet.
origin = pnts[i].copy()
depthVec = normals[i].copy()
depthVec.normalize()
depthVec.scaleBy(-depth)
origin.translateBy(depthVec)
zAxis = normals[i]
# Get a random direction angle.
angle = random.uniform(0, math.pi * 0.75)
# Create a temporary X vector using the random direction.
tempVec = adsk.core.Vector3D.create(math.cos(angle), math.sin(angle), angle)
# Compute the y axis.
yAxis = zAxis.crossProduct(tempVec)
yAxis.normalize()
# Compute the X axis.
xAxis = yAxis.crossProduct(zAxis)
xAxis.normalize()
trans = adsk.core.Matrix3D.create()
trans.setWithCoordinateSystem(origin, xAxis, yAxis, zAxis)
bodyCollection = adsk.core.ObjectCollection.create()
newGougeBody = gougeBody.copyToComponent(root)
bodyCollection.add(newGougeBody)
toolBodies.add(newGougeBody)
moveInput = root.features.moveFeatures.createInput(bodyCollection, trans)
root.features.moveFeatures.add(moveInput)
if (i % 25) == 0 and i != 0:
combineInput = root.features.combineFeatures.createInput(targetBody, toolBodies)
combineInput.targetBaseFeature = baseFeature
combineInput.operation = adsk.fusion.FeatureOperations.CutFeatureOperation
combineInput.isKeepToolBodies = False
combine = root.features.combineFeatures.add(combineInput)
toolBodies = adsk.core.ObjectCollection.create()
adsk.doEvents()
if toolBodies.count > 0:
combineInput = root.features.combineFeatures.createInput(targetBody, toolBodies)
combineInput.targetBaseFeature = baseFeature
combineInput.operation = adsk.fusion.FeatureOperations.CutFeatureOperation
combineInput.isKeepToolBodies = False
combine = root.features.combineFeatures.add(combineInput)
baseFeature.finishEdit()
ui.messageBox('Finished')
except:
if ui:
ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
def createPoints():
ui = None
try:
app = adsk.core.Application.get()
ui = app.userInterface
des = app.activeProduct
root = des.rootComponent
face = ui.selectEntity('Select a face', 'Faces').entity
meshCalc = face.meshManager.createMeshCalculator()
meshCalc.surfaceTolerance = 0.9
meshCalc.maxSideLength = 1
#meshCalc.maxAspectRatio = .9
mesh = meshCalc.calculate()
sk = root.sketches.add(root.xYConstructionPlane)
sk.isComputeDeferred = True
skPoints = sk.sketchPoints
coords = mesh.nodeCoordinatesAsDouble
result = ui.messageBox(str(len(coords)/3) + ' points will be created. Do you want to continue?', 'Continue?', adsk.core.MessageBoxButtonTypes.YesNoButtonType, adsk.core.MessageBoxIconTypes.QuestionIconType)
if result == adsk.core.DialogResults.DialogNo:
return
for i in range(0, mesh.nodeCount-1):
pnt1 = getPoint(coords, i)
skPoints.add(pnt1)
sk.isComputeDeferred = False
except:
if ui:
ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
def getPoint(array, index):
return adsk.core.Point3D.create(array[index*3], array[index*3+1], array[index*3+2])
