Split Body using multiple splitting tools

ChapmanM605 · ‎09-02-2024

Hi,

I am experienced on F360 but new to API, I have a tiny bit of Python knowledge so please forgive any rookie errors.

I am writing a script that splits a body into multiple, concentric cylinders. I want the script to be able to take limited inputs and then be able to conduct the process automatically from that data. For example - the spacing or pitch of the concentric cylinders determines how many there are within the start point (0,0,0) and outer radius decided by the user. I have managed to get this part to work correctly, a loop takes this information and sketches concentric circles on the end of a cylinder (1st picture). However, what I cant get to work is to be able to select all of the circle sketches as splitting tools which is allowed in the normal F360 design environment. (2nd picture) I have also tried to loop through each circle but that stops after the first split which I 'think' might be the fact that the original target body 'disappears' as it turns into two new bodies so loses its reference? This is the code version i include below but i have tried other ideas.

This is my code - forgive any rookie errors. Any help is appreciated on how i can efficiently, without needing to define and use every circle 'line by line' as a splitting tool, split the target body using all previously generated sketch circles.

Thank you

Matt

import adsk.core, adsk.fusion, traceback

import math

def run(context😞

ui = None

try:

app = adsk.core.Application.get()

ui = app.userInterface

doc = app.documents.add(adsk.core.DocumentTypes.FusionDesignDocumentType)

design = app.activeProduct

# Get the root component of the active design.

rootComp = design.rootComponent

# Get extrude features

extrudes = rootComp.features.extrudeFeatures

# Create a new sketch on the xy plane.

sketches = rootComp.sketches

xyPlane = rootComp.xYConstructionPlane

sketch = sketches.add(xyPlane)

Interval = 0.1

Outerradius = 5

Factor = 10

SInt = int(Interval * Factor)

SOR = int(Outerradius * Factor)

distance1 = adsk.core.ValueInput.createByReal(5)

radius = [(x+(Interval*Factor))/Factor for x in range(SInt,SOR,SInt)]

# Draw the circles.

circles = sketch.sketchCurves.sketchCircles

for r in radius:

circle1 = [circles.addByCenterRadius(adsk.core.Point3D.create(0, 0, 0), r)]

# Create a target body to use as a test case

sketch2 = sketches.add(xyPlane)

circles = sketch2.sketchCurves.sketchCircles

circle100 = circles.addByCenterRadius(adsk.core.Point3D.create(0, 0, 0), 10)

profile100 = sketch2.profiles.item(0)

extrude2 = extrudes.addSimple(profile100, distance1, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)

body = extrude2.bodies.item(0)

# Create SplitBodyFeatureInput

splitBodyFeats = rootComp.features.splitBodyFeatures

for x in circle1:

splitBodyInput = splitBodyFeats.createInput(body, x, True)

# Create split body feature

splitBodyFeats.add(splitBodyInput)

except:

if ui:

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

Jorge_Jaramillo · ‎09-03-2024

Hi,

The split body feature allows only to make it with a single tool at a time as it stated in the documentation:

In your code I fixed three errors you had:

1. circle1 was a list that kept just the last circle in the loop; need to be filled with every circle in the sketch.

2. splitBodyFeats.add() was called only at the end of the loop; need to be called for every split body input created.

3. body wasn't updated to keep the outer splitted part in preparation to the next split.

Here you have the script source code:

import adsk.core, adsk.fusion, traceback
import math

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

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

        # Get extrude features
        extrudes = rootComp.features.extrudeFeatures

        # Create a new sketch on the xy plane.
        sketches = rootComp.sketches
        xyPlane = rootComp.xYConstructionPlane
        sketch = sketches.add(xyPlane)

        Interval = 0.1
        Outerradius = 5
        Factor = 10
        SInt = int(Interval * Factor)
        SOR = int(Outerradius * Factor)
        distance1 = adsk.core.ValueInput.createByReal(5)

        radius = [(x+(Interval*Factor))/Factor for x in range(SInt,SOR,SInt)]
       
        # Draw the circles.
        circles = sketch.sketchCurves.sketchCircles
        # for r in radius:
        circle1 = [circles.addByCenterRadius(adsk.core.Point3D.create(0, 0, 0), r) for r in radius]
       
        # Create a target body to use as a test case
        sketch2 = sketches.add(xyPlane)
        circles = sketch2.sketchCurves.sketchCircles
        circle100 = circles.addByCenterRadius(adsk.core.Point3D.create(0, 0, 0), 10)
        profile100 = sketch2.profiles.item(0)
        extrude2 = extrudes.addSimple(profile100, distance1, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
         
        body = extrude2.bodies.item(0)
        # Create SplitBodyFeatureInput
        splitBodyFeats = rootComp.features.splitBodyFeatures
        for x in circle1:

            splitBodyInput = splitBodyFeats.createInput(body, x, True)
       
            # Create split body feature
            sbf = splitBodyFeats.add(splitBodyInput)
            body = sbf.bodies[1]
    except:
        # if ui:
        #     ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
        app.log('Failed:\n{}'.format(traceback.format_exc()))

Regards,

Jorge Jaramillo

ChapmanM605 · ‎09-03-2024

That is incredibly helpful, thank you for taking time to help!

Matt

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Split Body using multiple splitting tools

Split Body using multiple splitting tools

Split Body using multiple splitting tools