coilFeatures

[brad.bylls]

I see in the forum that the coil feature does not work in the API.

These were all dated back in 2016-2017

Has this been update?

And if so, could someone please show some code as to how to make a coil with the API?

I have a need to create springs and this would work perfectly.

Thank you.

[kandennti]

Hi @brad.bylls .

I recently made a sample of a coil.

https://forums.autodesk.com/t5/fusion-360-api-and-scripts/implementing-a-feature-similar-to-coil/m-p... 

Make the circle of the sketch selected beforehand and run next.　

app.executeTextCommand(u'Commands.Start Coil')

Then, after setting each item, run next.

app.executeTextCommand(u'NuCommands.CommitCmd')

However, I have not found a way to change anything other than these items.

'Rotation', which is not mentioned in the sample over there, can be manipulated in the following way.

app.executeTextCommand(u'Commands.SetBool CoilFlipRotation <0 or 1>')

Methods for performing functions that are not provided by the API are described in this section.

https://forums.autodesk.com/t5/fusion-360-api-and-scripts/use-textcommands2/td-p/9937161 

[brad.bylls]

Hi,

In another post you replied about using a pre-existing circle sketch which is exactly what I am trying to do.

I copied your script from my post and added your pre existing circle code and I get an error that the pre-existing circle is an "invalid argument entity"

The sketch is created with the circle.

#Fusion360API Python script

import adsk.core, adsk.fusion, traceback

import math

_app = adsk.core.Application.cast(None)

_ui = adsk.core.UserInterface.cast(None)

def run(context😞

    try:

        global _app, _ui

        _app = adsk.core.Application.get()

        _ui = _app.userInterface

        product = _app.activeProduct

        design = adsk.fusion.Design.cast(product)

        occs = design.rootComponent.occurrences

        mat = adsk.core.Matrix3D.create()

        newOcc = occs.addNewComponent(mat)

        newComp = adsk.fusion.Component.cast(newOcc.component)

        sketches = newComp.sketches

        xyPlane = newComp.xYConstructionPlane

        center = adsk.core.Point3D.create(0, 0, 0)

        # Create the body

        bodySketch = sketches.add(xyPlane)

        bodyCircle = bodySketch.sketchCurves.sketchCircles.addByCenterRadius(center, 1 * 2.54)

        # Coil parameters

        CoilDiameter = 10

        CoilPitch = 4

        CoilHeight = 30

        SectionSize = 1

        CoilFeatureType = 2

        CoilFeatureSectionType = 1

        # wait CommandIDs

        #waitLst = ('PrimitiveCoil','CircleCenterRadius')

        # call Coil command

        #_app.executeTextCommand(u'Commands.Start PrimitiveCoil')

        _ui.activeSelections.add(bodyCircle)  <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<

        _app.executeTextCommand(u'Commands.Start Coil')

        # wait

        while True:

            actCmd = _ui.activeCommand

            adsk.doEvents()

            if actCmd in waitLst:

                continue

            break

        # Cancel check

        if _ui.activeCommand != 'Coil':

            return

        # setting parameters

        cmds = [

            u'Commands.SetDouble SectionSize {}'.format(SectionSize),

            u'Commands.SetDouble CoilPitch {}'.format(CoilPitch),

            u'Commands.SetDouble CoilHeight {}'.format(CoilHeight),

            u'Commands.SetDouble CoilFeatureType {}'.format(CoilFeatureType)

            u'Commands.SetDouble CoilFeatureSectionType {}'.format(CoilFeatureSectionType)

        ]

        #[_app.executeTextCommand(cmd) for cmd in cmds]

        # command commit

        _app.executeTextCommand(u'NuCommands.CommitCmd')

    except:

        if _ui:

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

[kandennti · Accepted solution]

@brad.bylls .

I have not tried it, just looked at it a bit.

The most common reason for errors in Selections.Add is when the Occurrence entity is a nativeObject.

Although the content is different, I found a similar error here, so I created a sample.

https://forums.autodesk.com/t5/fusion-360-api-and-scripts/mesh-merge-feature-in-api/m-p/9940123#M121... 

I think you will have to use the createForAssemblyContext method.

[brad.bylls]

Thank you for the help but not working out as planned. I will go in another direction

[kandennti · Accepted solution]

@brad.bylls .

In the case of Occurrence entities, this will work.

・・・
        # call Coil command
        #_app.executeTextCommand(u'Commands.Start PrimitiveCoil')
        # _ui.activeSelections.add(bodyCircle)  <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
        proxy = bodyCircle.createForAssemblyContext(newOcc)
        _ui.activeSelections.add(proxy)
        _app.executeTextCommand(u'Commands.Start Coil')
・・・

[brad.bylls]

Thanks Kandennti, that worked.