Export profile sketch points to CSV

There is a Python script part of the Fusion 360 installation that can import points from a CSV file into a spline:

We could use the source code of that as a starting point to implement the reverse: export the points of a spline.

In this case, however, I'm changing it to export the points of a profile instead: one consisting of many short sketch lines forming a closed loop.

Because it's a closed loop, therefore it's enough to just export the coordinates of the start sketch point of each line as we iterate through the sketch lines. 

import adsk.core, adsk.fusion, traceback
import io

def run(context):
    ui = None
    try:
        app = adsk.core.Application.get()
        ui  = app.userInterface
        # Get all components in the active design.
        product = app.activeProduct
        design = adsk.fusion.Design.cast(product)
        title = 'Export Spline csv'
        if not design:
            ui.messageBox('No active Fusion design', title)
            return

        if app.userInterface.activeSelections.count != 1:
            ui.messageBox('Select profile before running command', title)
            return

        profile = app.userInterface.activeSelections.item(0).entity
        if not type(profile) is adsk.fusion.Profile:
            ui.messageBox('Selected object needs to be a profile', title)
            return

        dlg = ui.createFileDialog()
        dlg.title = 'Save CSV File'
        dlg.filter = 'Comma Separated Values (*.csv)'
        if dlg.showSave() != adsk.core.DialogResults.DialogOK :
            return
        
        filename = dlg.filename

        with io.open(filename, 'w', encoding='utf-8-sig') as f:
            profile = adsk.fusion.Profile.cast(profile)
            loop = profile.profileLoops.item(0)
            curves = loop.profileCurves
            for curve in curves:
                curve = adsk.fusion.ProfileCurve.cast(curve)
                entity = curve.sketchEntity
                point = entity.startSketchPoint
                point = adsk.fusion.SketchPoint.cast(point)
                geometry = point.geometry
                f.write(str(geometry.x) + "," + str(geometry.y) + "\n")

    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

In order to use the above code, you can simply create a new Python Script in the "Scripts and Add-Ins" dialog and replace the code in the generated Python file with the one shown above - see Creating a Script or Add-In  

Here is the result produced by the script:

-Adam