How Profiles in sketch are Index?

[design_kunalp]

I am Not good at programming only basic.

I am trying to extrude profile from sketch. 

sketch might be created by sketchLines && sketchCircles or by using DXF/CVS files data.

problem I faced is profile generated on same/identical sketch are index randomly every time I use Script.

maybe because sketch is defined in X-Y coordinate but sketching on yZConstructionPlane/Different Plane.

firstly, I thought Profile Indexing based on position from origin. then I thought based on Area of profile, small area index 0 to next. Both time there were two profiles at same distance from origin or have same area property. I didn't get any workaround for this.

it's like circle with two chords with same distance and normal to each other.

This will also help me with generating standard aluminum profiles but as I know their C/S area I find profile to extrude by inspecting their Area.

#Author- Kunal_Panchal
#Description- Aluminium Profiles Data form MiniTec

import adsk.core, adsk.fusion, adsk.cam, traceback

def run(context):
    ui = None
    try:
        app = adsk.core.Application.get()
        ui  = app.userInterface
        ui.messageBox("Addin By Kunal Panchal",'Aluminium Profiles',0,2)

        design = adsk.fusion.Design.cast(app.activeProduct)
        design.designType = adsk.fusion.DesignTypes.ParametricDesignType
        
        # Get import manager
        importManager = app.importManager
        
        # Get root component
        rootComp = design.rootComponent

        #sketches
        sketches = rootComp.sketches
        #sketch = sketches.add(app.activeProduct)

        #Getting User Inputs
        (Profile, cancelled) = ui.inputBox( "Profile Code:",'MiniTec Aluminium Profile')
        (Length, cancelled) = ui.inputBox( 'Length In MM:','Profile Length')
        Length = float(Length)/10

        #Removed Conditional Statements to simplify code but it gives following data.
        DXF_File = 'directory to dxffile'
        Profile_Code = 'Name of part Created'
        ExtrudedArea = 7.56 #Cross Section Area of Profile in cm^2 

        #Create DXF
        dxfOptions = importManager.createDXF2DImportOptions(DXF_File, rootComp.yZConstructionPlane)
        dxfOptions.isViewFit = True
        # Import dxf file to root component
        importManager.importToTarget(dxfOptions, rootComp)

        #Find Sketch to Extrude
        sketch_avi = sketches.count
        sketch = design.rootComponent.sketches.item(sketch_avi-1)
        extrudes = rootComp.features.extrudeFeatures
        extrudedist = adsk.core.ValueInput.createByReal(Length)

        #To find Profile that Need to Extrude
        Area = []
        profile_avi = sketch.profiles.count
        for i in range(0,profile_avi):
            Inspect_Profile = sketch.profiles.item(i)
            areaProps = Inspect_Profile.areaProperties()
            area = areaProps.area
            Area.append(round(area, 2))
            #ui.messageBox(str(Area)) #For Debugging/Calculating area of each profile avilable in sketch

        prof = sketch.profiles.item(Area.index(ExtrudedArea))
        extrude = extrudes.addSimple(prof, extrudedist, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
        body1 = extrude.bodies.item(0)
        body1.name = Profile_Code
        ui.messageBox(Profile_Code+' Created','MiniTec Profile',0,2)
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

I their another way to optimize this and again if I know how profile are index, I don't need to inspect profiles in loop. 

[kandennti · Accepted solution]

Hi @design_kunalp .

There are many possible ways to do this, but why not find a profile that matches the area?

・・・
        extrudedist = adsk.core.ValueInput.createByReal(Length)

        # Get Profile to Extrude
        profs = get_profiles_by_area(
            sketch,
            ExtrudedArea
        )
        if len(profs) < 1:
            return

        # Create Extrude
        prof: adsk.fusion.Profile = None
        for prof in profs:
            extrude: adsk.fusion.ExtrudeFeature = extrudes.addSimple(
                prof,
                extrudedist,
                adsk.fusion.FeatureOperations.NewBodyFeatureOperation
            )
            extrude.bodies.item(0).name = Profile_Code

        ui.messageBox(Profile_Code+' Created','MiniTec Profile',0,2)
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))


def get_profiles_by_area(
    sketch: adsk.fusion.Sketch,
    targetArea: float,
    tolerance: float = 0.001,
) -> list[adsk.fusion.Profile]:

    if sketch.profiles.count < 1:
        return []

    profs = []
    prof: adsk.fusion.Profile = None
    for prof in sketch.profiles:
        areaProps: adsk.fusion.AreaProperties = prof.areaProperties()
        print(areaProps.area)
        if abs(targetArea - areaProps.area) < tolerance:
            profs.append(prof)

    return profs

[kandennti · Accepted solution]

If you know that they are the two smallest Areas in the profile, sort by Area and push out only two.

・・・
        extrudedist = adsk.core.ValueInput.createByReal(Length)

        # Get list of profiles sorted by Area
        profs = sorted(sketch.profiles, key =lambda x: x.areaProperties().area)

        # Create Extrude
        extrude: adsk.fusion.ExtrudeFeature = extrudes.addSimple(
            lst_to_objs(profs[:2]),
            extrudedist,
            adsk.fusion.FeatureOperations.NewBodyFeatureOperation
        )
        body: adsk.fusion.BRepBody = None
        for body in extrude.bodies:
            body.name = Profile_Code

        ui.messageBox(Profile_Code+' Created','MiniTec Profile',0,2)
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))


def lst_to_objs(
    profs: list[adsk.fusion.Profile]
) -> adsk.core.ObjectCollection:

    objs: adsk.core.ObjectCollection = adsk.core.ObjectCollection.create()
    [objs.add(p) for p in profs]

    return objs

[sylvain_boyer6TGNB]

I am in the same situation and the solution above was helpful. However it failed with large profiles, extruding the voids of my profile.
I used the code snippet but modified it a little bit to use the perimeter of the profile rather the area.