Mouse Click Event

[Anonymous]

Hi.

I made a command which have button1 and textBox1.

I want to add a following mouse click event.

1. Click button1.(get-point mode is activated.)

2. Click any point of coordinates.

3. Get the point vector and write it to textBox1.

Could you help me with this problem? or give me a example of mouse click event?

Thank you.

[ekinsb]

I just finished writing a little sample for this and have discovered a problem with the mouse click event where it's not being fired correctly.  Until it's fixed you can possibly make do with the mouse up event instead.  However, you need to be aware of what the event is actually giving you to see if any of these can meet your needs.  The mouse related events return the current position of the mouse in window coordinates.  These are 2D coordinates where (0,0) is the upper-left corner of the main Fusion window.  There isn't an equivalent 3D point available.  However, if there was, it's position is somewhat arbitrary because two positions are defined by the mouse but the depth in 3D space is undefined.

[Anonymous]

When I click the button something like 'Box', (1) I can select a plane, and (2) choice a point on the plane.

Is there a API to do like that?

[ekinsb]

You can do the selection of something using a SelectionCommandInput.  This returns a Selection object which provides access to the entity that was selected and also the point where it was selected.  We're missing the ability to just have a mouse point specified and is something we need to look at adding to the API.

[MichaelT_123]

G'day Mr. Ekins,

I have difficult problem, which needs simple solution. 😉

I want to differentiate, which mouse button is used when clicking on button box.

You have mentioned that there is an implementation issue with MouseEventHandler family.

Has the issue been resolved?

Regards

MichaelT

[ekinsb]

When a button, or any command input, is interacted with on a command dialog the API only reports which command input was interacted with and not how it was interacted with.  I've never heard this requirement before and am curious why you want to do something like that. 

[MichaelT_123]

G'Night Mr. Ekins

... I just want(ed) create quick "snap/unsnap" trigger mechanisms using right and left button on the mouse. Possibly other ideas could be realised ... who knows.

I have to say, it is not a critical problem ... I can live without it's resolution, ... but I am curious ..  :).

I have used as a template the sample code from API doc. The one adding button on ToolBar_QAT

I have modified it slightly and it has been working just fine. Unfortunately, bad on me, one night I had an Idea ..."Why not devote the right mouse button for a specific function?" 

And as usual  ... curiosity struck back !

Here is a snipet of code dealing of adding handler function to command definition together with the str(Handlers) themselves and resulting error log.

----------------------------------------------------------------------------------------------------

try:

    onMouseClick = MyMouseClickHandler()       #Vanila/minimal definition

    onMouseClickStr = str(onMouseClick)

    cmdDefinition_SSnap.mouseClick.add(onMouseClick)

    handlers.append(onMouseClick)

    ui.messageBox(_('MyMouseClickHandler() command created successfully'))

except:

   errorStr = _('QAT command created failed: {}').format(traceback.format_exc())

   ui.messageBox(_('QAT command created failed: {}').format(traceback.format_exc()))

   exit()

---------------------------------------------------------------

<__main__C%3A%2FFusion360%2FAPI%2FAddIns%2FSSnap%2FSSnap_py.CommandCreatedEventHandlerQAT; proxy of <Swig Object of type 'adsk::core::CommandCreatedEventHandler *' at 0x000000A717FCA780> >
<__main__C%3A%2FFusion360%2FAPI%2FAddIns%2FSSnap%2FSSnap_py.MyMouseClickHandler; proxy of <Swig Object of type 'adsk::core::MouseEventHandler *' at 0x000000A717FCA7B0> >

QAT command created failed: Traceback (most recent call last):
File ".\Ssnap.py", line 260, in run
cmdDefinition_SSnap.mouseClick.add(onMouseClick)
File "…\adsk\core.py", line 3757, in <lambda>
__getattr__ = lambda self, name: _swig_getattr(self, CommandDefinition, name)
File "…\adsk\core.py", line 57, in _swig_getattr
raise AttributeError(name)
AttributeError: mouseClick

-------------------------------------------------------------------------------------

With Regards

MichaelT

PS. As I mentioned, please don't bother too much ... it is not a serious problem ... there is also possibility that I did something stupid ... so if you will point it out ... I will be delighted!

[brad.bylls]

You mention with SelectionCommandInput you can get a face and the point where selected.

This exactly what I am looking for. 

I want the user to select a planar face and that face will be the sketch plane and the selection point the center of a circle. 

Is there some sample code somewhere that shows how to do this? 

Thank you. 

[kandennti]

Hi @brad.bylls .

I made a sample.

import adsk.core, adsk.fusion, traceback

def run(context):
    ui = None
    try:
        app = adsk.core.Application.get()
        ui = app.userInterface

        design = app.activeProduct
        rootComp = design.rootComponent
        sketches :adsk.fusion.Sketches = rootComp.sketches

        # select PlanarFaces
        try:
            returnValue :adsk.core.Selections = ui.selectEntity(
                'Select Face', 'PlanarFaces')
        except:
            return

        # Selected surface
        surf :adsk.fusion.BRepFace = returnValue.entity
        
        # Create Sketch
        skt :adsk.fusion.Sketch = sketches.add(surf)

        # Click Point
        pnt :adsk.core.Point3D = returnValue.point

        # Get the difference between the RootComponent and the origin of the sketch.
        mat :adsk.core.Matrix3D = skt.transform

        # Inverts this matrix.
        mat.invert()

        # Convert the difference
        pnt.transformBy(mat)

        # Draw Sketch
        radius = 2.0
        circles :adsk.fusion.SketchCircles = skt.sketchCurves.sketchCircles
        circles.addByCenterRadius(pnt, radius)
    except:
        if ui:
            ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

[brad.bylls]

This is my code using your sample.

It goes through the ui.selectentity code, but doesn't stop to get the face and returns out of the code.

def drawBolt(design, numBushingID, numBushingOD, numBushingLength, numClearLength, numHeadDiam, numHeadHeight😞

    ui = None

    try:

        # Create a new component by creating an occurrence.

        occs = design.rootComponent.occurrences

        mat = adsk.core.Matrix3D.create()

        newOcc = occs.addNewComponent(mat)

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

        ui = adsk.core.UserInterface

        # Everthing here expects all distances to be in centimeters,

        # so convert for the bolt creation.

        sizeUnits = 2.54

        numClearDiam = (numBushingID + .125) * sizeUnits

        numBushingID = numBushingID * sizeUnits

        numPressDiam = (numBushingOD - .0005) * sizeUnits

        numBushingOD = numBushingOD * sizeUnits

        numBushingLength = numBushingLength * sizeUnits

        numCboreDiam = (numHeadDiam + .01) * sizeUnits

        numHeadDiam = numHeadDiam * sizeUnits

        numHeadHeight = numHeadHeight * sizeUnits

        numClearLength = numClearLength * sizeUnits

        try:

            returnValue :adsk.core.Selections = ui.selectEntity(

                'Select Face', 'PlanarFaces')

        except:

            return  <<<<< executes to here and exits

        xyPlane :adsk.fusion.BRepFace = returnValue.entity

        xyPlane :adsk.fusion.Sketch = sketches.add(xyPlane)

        pnt :adsk.core.Point3D = returnValue.point

        mat :adsk.core.Matrix3D = xyPlane.transform

        mat.invert()

        pnt.transformBy(mat)

        # create the head

        headSketch = sketches.add(xyPlane)

        headCircle = headSketch.sketchCurves.sketchCircles.addByCenterRadius(center, numHeadDiam / 2)

        headSketch.sketchDimensions.addDiameterDimension(headCircle, adsk.core.Point3D.create(1, 1, 0))

        headSketch.name = 'Head Diameter Sketch'

        extrudes = newComp.features.extrudeFeatures

        headProf = headSketch.profiles[0]

        headExtInput = extrudes.createInput(headProf, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)

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

        headExtInput.setDistanceExtent(False, distance1)

        headExt = extrudes.add(headExtInput)

        headExt.name = 'Head Height'

        # Create the OD body

        bushingOdSketch = sketches.add(xyPlane)

        bushingOdCircle = bushingOdSketch.sketchCurves.sketchCircles.addByCenterRadius(center, numBushingOD / 2)

        bushingOdSketch.sketchDimensions.addDiameterDimension(bushingOdCircle, adsk.core.Point3D.create(1, 0, 0))

        bushingOdSketch.name = 'O.D. Sketch'

        bushingOdProf = bushingOdSketch.profiles[0]

        bushingOdExtInput = extrudes.createInput(bushingOdProf, adsk.fusion.FeatureOperations.JoinFeatureOperation)

        distance2 = adsk.core.ValueInput.createByReal(numBushingLength)

        bushingOdExtInput.setDistanceExtent(False, distance2)

        bushingOdExt = extrudes.add(bushingOdExtInput)

        bushingOdExt.name = 'Bushing Length'

        # Create the ID cut

        bushingIdSketch = sketches.add(xyPlane)

        bushingIdCircle = bushingIdSketch.sketchCurves.sketchCircles.addByCenterRadius(center, numBushingID / 2)

        bushingIdSketch.sketchDimensions.addDiameterDimension(bushingIdCircle, adsk.core.Point3D.create(1, 1, 0))

        bushingIdSketch.name = 'I.D. Sketch'

        bushingIdProf = bushingIdSketch.profiles[0]

        bushingIdExtInput = extrudes.createInput(bushingIdProf, adsk.fusion.FeatureOperations.CutFeatureOperation)

        distance3 = adsk.core.ValueInput.createByReal(numBushingLength)

        bushingIdExtInput.setDistanceExtent(False, distance3)

        bushingIdExtInput.participantBodies = [bushingOdExt.bodies.item(0)]

        bushingIdExt = extrudes.add(bushingIdExtInput)

        bushingIdExt.name = 'Bushing Length'

        # Create the bushing fillet

        bushingEnds = bushingOdExt.endFaces.item(0)

        filletEdge = bushingEnds.edges.item(0)

        edgeCol = adsk.core.ObjectCollection.create()

        edgeCol.add(filletEdge)

        filletFeats = newComp.features.filletFeatures

        filletInput = filletFeats.createInput()

        filletSize = adsk.core.ValueInput.createByReal(.254)

        filletInput.addConstantRadiusEdgeSet(edgeCol, filletSize, True)

        newFilletFeats = filletFeats.add(filletInput)

        newFilletFeats.name = 'Fillet'

        # Name the body

        fc = bushingOdExt.faces[0]

        bd = fc.body

        bd.name = _inputCatalogNumber.text + ' Bushing'

        fusionMaterials = _app.materialLibraries.itemByName('Fusion 360 Appearance Library')

        appear = fusionMaterials.appearances.itemByName('Powder Coat (Blue)')

        bd.appearance = appear

        # Group everything used to create the bushing body in the timeline.

        bushingTimelineGroups = design.timeline.timelineGroups

        bushingOccIndex = newOcc.timelineObject.index

        filletFeatsIndex = newFilletFeats.timelineObject.index

        bushingTimelineGroup = bushingTimelineGroups.add(bushingOccIndex, filletFeatsIndex)

        bushingTimelineGroup.name = _inputCatalogNumber.text + ' Bushing'

        # Create a clearance length extrude. Used in parameter expressions

        clearanceLengthSketch = sketches.add(xyPlane)

        clearanceLengthCircle = clearanceLengthSketch.sketchCurves.sketchCircles.addByCenterRadius(center, .01)

        clearanceLengthSketch.name = 'Clearance Length Sketch'

        clearanceLengthProf = clearanceLengthSketch.profiles[0]

        clearanceLengthExtInput = extrudes.createInput(clearanceLengthProf, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)

        distance3 = adsk.core.ValueInput.createByReal(numClearLength * -1)

        clearanceLengthExtInput.setDistanceExtent(False, distance3)

        clearanceLengthExt = extrudes.add(clearanceLengthExtInput)

        clearanceLengthExt.name = 'Clearance Length'

        clearanceLengthExt.isSuppressed = True

        # Create the bushing press fit

        cutBushingSketch = sketches.add(xyPlane)

        cutBushingCircle = cutBushingSketch.sketchCurves.sketchCircles.addByCenterRadius(center, numPressDiam / 2)

        cutBushingSketch.sketchDimensions.addDiameterDimension(cutBushingCircle, adsk.core.Point3D.create(0, 1, 0))

        cutBushingSketch.name = 'Bushing Press Fit Sketch'

        cutBushingProf = cutBushingSketch.profiles[0]

        cutBushingExtInput = extrudes.createInput(cutBushingProf, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)

        distance4 = adsk.core.ValueInput.createByReal(numBushingLength)

        cutBushingExtInput.setDistanceExtent(False, distance4)

        cutBushingExt = extrudes.add(cutBushingExtInput)

        cutBushingExt.name = 'Bushing Press Fit'

        # Create the head clearance

        cutHeadSketch = sketches.add(xyPlane)

        cutHeadCircle = cutHeadSketch.sketchCurves.sketchCircles.addByCenterRadius(center, numCboreDiam / 2)

        cutHeadSketch.sketchDimensions.addDiameterDimension(cutHeadCircle, adsk.core.Point3D.create(-1, 1, 0))

        cutHeadSketch.name = 'Head Clearance Sketch'

        cutHeadProf = cutHeadSketch.profiles[0]

        cutHeadExtInput = extrudes.createInput(cutHeadProf, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)

        distance5 = adsk.core.ValueInput.createByReal(numHeadHeight)

        cutHeadExtInput.setDistanceExtent(False, distance5)

        cutHeadExt = extrudes.add(cutHeadExtInput)

        cutHeadExt.name = 'Head Clearance Length'

        # Create the bushing clearance hole

        cutBushingClearSketch = sketches.add(xyPlane)

        cutBushingClearCircle = cutBushingClearSketch.sketchCurves.sketchCircles.addByCenterRadius(center, numClearDiam / 2)

        cutBushingClearSketch.sketchDimensions.addDiameterDimension(cutBushingClearCircle, adsk.core.Point3D.create(-1, 0, 0))

        cutBushingClearSketch.name = 'Bushing Clearance Sketch'

        cutBushingClearProf = cutBushingClearSketch.profiles[0]

        cutBushingClearExtInput = extrudes.createInput(cutBushingClearProf, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)

        distance6 = adsk.core.ValueInput.createByReal(numClearLength * -1)

        cutBushingClearExtInput.setDistanceExtent(False, distance6)

        cutBushingClearExt = extrudes.add(cutBushingClearExtInput)

        cutBushingClearExt.name = 'Bushing Clearance Length'

        # Create cut body with combine

        cutBody = cutBushingExt.bodies[0]

        bodyCollection = adsk.core.ObjectCollection.create()

        bodyCollection.add(cutHeadExt.bodies[0])

        bodyCollection.add(cutBushingClearExt.bodies[0])

        model = design.activeComponent

        features = model.features

        combineFeat = features.combineFeatures

        combineInput = combineFeat.createInput(cutBody, bodyCollection)

        combineFeatur = combineFeat.add(combineInput)

        # Name the cut body

        fc = combineFeatur.faces[0]

        bd = fc.body

        bd.name = 'Bushing Cut Body'

        fusionMaterials = _app.materialLibraries.itemByName('Fusion 360 Appearance Library')

        appear = fusionMaterials.appearances.itemByName('Powder Coat (Green)')

        bd.appearance = appear

        # Group everything used to create the bushing cut body in the timeline.

        cutTimelineGroups = design.timeline.timelineGroups

        cutOccIndex = clearanceLengthSketch.timelineObject.index

        combineFeatIndex = combineFeatur.timelineObject.index

        cutTimelineGroup = cutTimelineGroups.add(cutOccIndex, combineFeatIndex)

        cutTimelineGroup.name = _inputCatalogNumber.text + ' Cut Body'

        # Add an attribute to the component with all of the input values.  This might

        # be used in the future to be able to edit the bushing.

        bushingValues = {}

        bushingValues['bushingID'] = str(numBushingID)

        bushingValues['bushingOD'] = str(numBushingOD)

        bushingValues['bushingLength'] = str(numBushingLength)

        bushingValues['headDiameter'] = str(numHeadDiam)

        bushingValues['headHeight'] = str(numHeadHeight)

        bushingValues['catalogNumber'] = _inputCatalogNumber

        attrib = newComp.attributes.add('CreateShbu', 'Values', str(bushingValues))

        newComp.name = _inputCatalogNumber.text + ' Guide Bushing'

        return newComp

    except:

        if ui:

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

[kandennti]

I have not tried, but perhaps this is the cause.

・・・
        newOcc = occs.addNewComponent(mat)
        newComp = adsk.fusion.Component.cast(newOcc.component)
        ui :adsk.core.UserInterface = adsk.core.Application.get().userInterface #<-here

        # Everthing here expects all distances to be in centimeters,
        # so convert for the bolt creation.
・・・

[brad.bylls]

Sorry, when it gets to this line:

returnValue :adsk.core.Selections = ui.selectEntity(

                'Select Face', 'PlanarFaces')

It locks up F360

I have to go into the task manager and kill it.

[brad.bylls]

From what I am seeing in other posts, there is a problem with selectEntity in a addin but not in a plain script.

Do you know how to do this with selectCommandInput?

[kandennti]

I think it would work if we stopped selecting in the drawBolt function and received the face and point as parameters of the function.

# https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-4fbdc9ad-1dd4-4dca-bdf1-0000cbfe10d9
class MyExecuteHandler(adsk.core.CommandEventHandler):
    def __init__(self):
        super().__init__()
    def notify(self, args):
        eventArgs = adsk.core.CommandEventArgs.cast(args)

        # https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-e02e3629-e849-4881-92dc-f6f92bcffced
        selection_var = selectionCommandInput_var.selection(0)

        # https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-5b91bbc5-c644-4405-b462-08930de210f9
        selectPlanarFace = selection_var.entity

        # https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-c6307268-d1b4-4cbe-92e7-ed43c24562f2
        clickPoint = selection_var.point

        # call function
        def drawBolt(design_var, ・・・・, selectPlanarFace, clickPoint)


def drawBolt(
    design, 
    numBushingID, 
    numBushingOD, 
    numBushingLength, 
    numClearLength, 
    numHeadDiam, 
    numHeadHeight,
    xyPlane :adsk.fusion.BRepFace,
    pnt :adsk.core.Point3D):

・・・

[brad.bylls]

No go.

Still locks up on the selectEntity line in the addin.

        _ui.messageBox('Select A Face to Place Bushing')

        selectionCommandInput_var = _ui.selectEntity('Select a Face', 'PlanarFaces')

        selection_var = selectionCommandInput_var.selection(0)

        selectPlanarFace = selection_var.entity

        clickPoint = selection_var.point

        # Create the bolt.

        boltComp = drawBolt(des, numBushingID, numBushingOD, numBushingLength, numClearLength, \

                    numHeadDiam, numHeadHeight, selectPlanarFace, clickPoint)

[brad.bylls]

Got it.

Disregard my last reply.

Thank you so much.

[brad.bylls]

Hello,

I thought I had it working but the 3DPoint values comes back in cm's I think.

How can I change the x,y,z values of the 3DPoint to inches?

[BrianEkins]

The internal units for length inside Fusion is centimeters and the API uses these same units.  You can read more about this in the API user manual (http://help.autodesk.com/view/fusion360/ENU/?guid=GUID-A81B295F-984A-4039-B1CF-B449BEE893D7).