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Project To Surface API Sample

Description

Projects the specified set of curves onto the specified set of faces using the specified method of projection.

Code Samples 

import adsk.core, adsk.fusion, traceback

def run(context):
    ui = None
    try:
        app = adsk.core.Application.get()
        ui = app.userInterface
        
        # Create a document.
        doc = app.documents.add(adsk.core.DocumentTypes.FusionDesignDocumentType)
 
        product = app.activeProduct
        design = adsk.fusion.Design.cast(product)

        # Get the root component of the active design
        rootComp = design.rootComponent

        allOccs = rootComp.occurrences
        transform = adsk.core.Matrix3D.create()
        
        # Create three components under root component
        occ1 = allOccs.addNewComponent(transform)
        subComp1 = occ1.component
        occ2 = allOccs.addNewComponent(transform)
        subComp2 = occ2.component
        occ3 = allOccs.addNewComponent(transform)
        subComp3 = occ3.component
      
        # Create a sketch in sub component 1
        sketches1 = subComp1.sketches
        sketch1 = sketches1.add(rootComp.yZConstructionPlane)
        
        # Get sketch lines
        sketchLines = sketch1.sketchCurves.sketchLines
        
        # Create sketch rectangle
        startPoint = adsk.core.Point3D.create(-8.0, 0, 0)
        endPoint = adsk.core.Point3D.create(8.0, 8.0, 0)
        sketchLines.addTwoPointRectangle(startPoint, endPoint)
        
        # Get the profile of the first sketch
        prof1 = sketch1.profiles.item(0)
        
        # Create an extrusion input
        extrudes1 = subComp1.features.extrudeFeatures
        extInput1 = extrudes1.createInput(prof1, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        
        # Define that the extent is a distance extent of 2 cm
        distance1 = adsk.core.ValueInput.createByReal(2.0)
        # Set the distance extent
        extInput1.setDistanceExtent(False, distance1)
        # Set the extrude type to be solid
        extInput1.isSolid = True
        
        # Create the extrusion
        ext1 = extrudes1.add(extInput1)
        
        # Create construction plane
        planes = rootComp.constructionPlanes
        planeInput = planes.createInput()
        offsetValue = adsk.core.ValueInput.createByReal(8.0)
        planeInput.setByOffset(rootComp.yZConstructionPlane, offsetValue)
        plane = planes.add(planeInput)

         # Create a sketch in sub component 2
        sketches2 = subComp2.sketches
        sketch2 = sketches2.add(plane)
        
        # Create the spline.
        points = adsk.core.ObjectCollection.create()
        points.add(adsk.core.Point3D.create(0, 8, 0))
        points.add(adsk.core.Point3D.create(5, 6, 0))
        points.add(adsk.core.Point3D.create(-5, 5, 0))
        
        sketch2Curves = sketch2.sketchCurves
        spline = sketch2Curves.sketchFittedSplines.add(points)
        
        # Create sketch rectangle
        sketch2Lines = sketch2Curves.sketchLines
        startPoint2 = adsk.core.Point3D.create(-4, 2, 0)
        endPoint2 = adsk.core.Point3D.create(3, 4, 0)
        sketch2Lines.addTwoPointRectangle(startPoint2, endPoint2)
        
        # Get the profile of the second sketch
        prof2 = sketch2.profiles.item(0)
        
        # Create an extrusion input       
        extrudes2 = subComp2.features.extrudeFeatures
        extInput2 = extrudes2.createInput(prof2, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        
        # Define that the extent is a distance extent of 2 cm
        extent_distance_2 = adsk.fusion.DistanceExtentDefinition.create(adsk.core.ValueInput.createByString("2cm"))
        # Define that the taple angle is 10 degree
        deg10 = adsk.core.ValueInput.createByString("10 deg")

        extInput2.setOneSideExtent(extent_distance_2, adsk.fusion.ExtentDirections.PositiveExtentDirection, deg10)
        
        # Set the extrude type to be solid
        extInput2.isSolid = True

        # Create the extrusion
        ext2 = extrudes2.add(extInput2)
        
        # Get the body with the first extrude
        body = ext1.bodies.item(0)
        
        # Get faces
        faceList = []
        for face in body.faces:
            faceList.append(face)

        # Get curves
        curveList = []
        for curve in sketch2Curves:
            curveList.append(curve)
        
        # Get points
        for point in sketch2.sketchPoints:
            curveList.append(point)
        
        # Get the body with the second extrude
        body2 = ext2.bodies.item(0)
        
        # Get eges
        for edge in body2.edges:
            curveList.append(edge)
        
        # Get construction axis
        curveList.append(rootComp.yConstructionAxis)
        
        # Get construction point
        curveList.append(rootComp.originConstructionPoint)
        
        sketches3 = subComp3.sketches
        # Create a sketch in sub component 3
        skAlongVecProject = sketches3.add(rootComp.yZConstructionPlane)
        # sketch project to surface (along vector)
        projectedEntities = skAlongVecProject.projectToSurface(faceList, curveList, adsk.fusion.SurfaceProjectTypes.AlongVectorSurfaceProjectType, rootComp.xConstructionAxis)

        projectedEntities = []
        # Create a sketch in sub component 3
        skClosestPtProject = sketches3.add(rootComp.yZConstructionPlane)
        # sketch project to surface (closest point)
        projectedEntities = skClosestPtProject.projectToSurface(faceList, curveList, adsk.fusion.SurfaceProjectTypes.ClosestPointSurfaceProjectType)
        
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))


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