Multi chamfer problems

[brad.bylls]

Trying to chamfer three edges on a component.

328    # Create the chamfer
329    edgeCol = adsk.core.ObjectCollection.create()
330    edgeCol.clear()
331    edges = stemExt.sideFaces[0].edges # I've tried [1] and [2] also
332    for edgeI in edges:
333        edgeCol.add(edgeI)
334
335    chamferFeats = newComp.features.chamferFeatures
336    chamferInput = chamferFeats.createInput(edgeCol, True)
337    chamferInput.setToEqualDistance(
338        adsk.core.ValueInput.createByReal((numStemDiam - numHoleThru)/4))
339    chamferFeats.add(chamferInput)

I get this error

[BrianEkins]

Can you post the model? I created a model that looks similar and it works for me.

[Jorge_Jaramillo]

@Jorge_Jaramillo - this post is being edited to remove PII.

Hi,

Just to be sure you are in the correct feature, could you check :

stemExt.sideFaces.count

If it is > 1 then can you try with instead:

edges = stemExt.sideFaces.item(0).edges

Could you share how it creates stemExt feature?  What kind of feature is stemExt?

Regards,

Jorge Jaramillo

[brad.bylls]

 # Create the stem
    stemSketch = sketches.addWithoutEdges(xyPlane)
    center = stemSketch.modelToSketchSpace(clickPoint)
    stemCircle = stemSketch.sketchCurves.sketchCircles.addByCenterRadius(center, numStemDiam/2)
    stemSketch.sketchDimensions.addDiameterDimension(stemCircle, adsk.core.Point3D.create(1, 0, 0))
    stemSketch.name = 'Stem Diameter Sketch'
    stemProf = stemSketch.profiles[0]
    stemExtInput = extrudes.createInput(stemProf, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
    distance3 = adsk.core.ValueInput.createByReal(numStemLen + numHexLen + numThreadStraight)
    stemExtInput.setDistanceExtent(False, distance3)
    stemExt = extrudes.add(stemExtInput)
    # Change to inches in Parameters
    extent_3 = stemExt.extentOne
    distanceMP_3 = extent_3.distance
    distanceMP_3.expression = "{:.{}f}".format(((numStemLen + numHexLen + numThreadStraight) / sizeUnits), 4) + 'in'
    # Add the name
    stemExt.name = 'Stem length from face'

    # Create the oil groove
    stemGrooveSketch = sketches.addWithoutEdges(xyPlane)
    stemGrooveCircle = stemGrooveSketch.sketchCurves.sketchCircles.addByCenterRadius(
        center, (numStemDiam + .1) / 2)
    stemGrooveCircle1 = stemGrooveSketch.sketchCurves.sketchCircles.addByCenterRadius(
        center, (numStemDiam-(numStemDiam - numHoleThru)/2) / 2)
    stemGrooveSketch.sketchDimensions.addDiameterDimension(stemGrooveCircle, adsk.core.Point3D.create(1, 1, 0))
    stemGrooveSketch.name = 'Stem Groove Sketch'
    stemGrooveProf = stemGrooveSketch.profiles[0]
    stemGrooveExtInput = extrudes.createInput(stemGrooveProf, adsk.fusion.FeatureOperations.CutFeatureOperation)
    grooveCenter = (numThreadStraight + numHexLen + (numStemLen / 2)) * -1
    distance11 = adsk.fusion.DistanceExtentDefinition.create(
        adsk.core.ValueInput.createByReal((grooveCenter + .05) * -1))
    distance11A = adsk.fusion.DistanceExtentDefinition.create(
        adsk.core.ValueInput.createByReal(grooveCenter - .05))
    deg0 = adsk.core.ValueInput.createByString("0 deg")
    stemGrooveExtInput.setTwoSidesExtent(distance11, distance11A, deg0, deg0)
    stemGrooveExtInput.participantBodies = [stemExt.bodies.item(0)]
    stemGrooveExt = extrudes.add(stemGrooveExtInput)
    # Change to inches in Parameters
    extent_11A = stemGrooveExt.extentOne
    extent_11B = stemGrooveExt.extentTwo
    distanceMP_11A = extent_11A.distance
    distanceMP_11B = extent_11B.distance
    distanceMP_11A.expression = "{:.{}f}".format((((grooveCenter + .05) * -1) / sizeUnits), 4) + 'in'
    distanceMP_11B.expression = "{:.{}f}".format(((grooveCenter + .05) / sizeUnits), 4) + 'in'
    stemGrooveExt.name = 'Stem Groove'

    # Create body with combine
    plugBody = plugExt.bodies[0]
    bodyCollection = adsk.core.ObjectCollection.create()
    bodyCollection.add(plugStraightExt.bodies[0])
    bodyCollection.add(hexExt.bodies[0])
    bodyCollection.add(stemExt.bodies[0])
    model = design.activeComponent
    features = model.features
    combineFeat = features.combineFeatures
    combineInput = combineFeat.createInput(plugBody, bodyCollection)
    combineFeatur = combineFeat.add(combineInput)

    # Create the chamfer
    edgeCol = adsk.core.ObjectCollection.create()
    edgeCol.clear()
    edges = stemExt.sideFaces.item(0).edges
    for edgeI in edges:
        edgeCol.add(edgeI)

    chamferFeats = newComp.features.chamferFeatures
    chamferInput = chamferFeats.createInput(edgeCol, True)
    chamferInput.setToEqualDistance(
        adsk.core.ValueInput.createByReal((numStemDiam - numHoleThru)/4))
    chamferFeats.add(chamferInput)

[brad.bylls]

 # Create the stem
    stemSketch = sketches.addWithoutEdges(xyPlane)
    center = stemSketch.modelToSketchSpace(clickPoint)
    stemCircle = stemSketch.sketchCurves.sketchCircles.addByCenterRadius(center, numStemDiam/2)
    stemSketch.sketchDimensions.addDiameterDimension(stemCircle, adsk.core.Point3D.create(1, 0, 0))
    stemSketch.name = 'Stem Diameter Sketch'
    stemProf = stemSketch.profiles[0]
    stemExtInput = extrudes.createInput(stemProf, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)
    distance3 = adsk.core.ValueInput.createByReal(numStemLen + numHexLen + numThreadStraight)
    stemExtInput.setDistanceExtent(False, distance3)
    stemExt = extrudes.add(stemExtInput)
    # Change to inches in Parameters
    extent_3 = stemExt.extentOne
    distanceMP_3 = extent_3.distance
    distanceMP_3.expression = "{:.{}f}".format(((numStemLen + numHexLen + numThreadStraight) / sizeUnits), 4) + 'in'
    # Add the name
    stemExt.name = 'Stem length from face'

    # Create the oil groove
    stemGrooveSketch = sketches.addWithoutEdges(xyPlane)
    stemGrooveCircle = stemGrooveSketch.sketchCurves.sketchCircles.addByCenterRadius(
        center, (numStemDiam + .1) / 2)
    stemGrooveCircle1 = stemGrooveSketch.sketchCurves.sketchCircles.addByCenterRadius(
        center, (numStemDiam-(numStemDiam - numHoleThru)/2) / 2)
    stemGrooveSketch.sketchDimensions.addDiameterDimension(stemGrooveCircle, adsk.core.Point3D.create(1, 1, 0))
    stemGrooveSketch.name = 'Stem Groove Sketch'
    stemGrooveProf = stemGrooveSketch.profiles[0]
    stemGrooveExtInput = extrudes.createInput(stemGrooveProf, adsk.fusion.FeatureOperations.CutFeatureOperation)
    grooveCenter = (numThreadStraight + numHexLen + (numStemLen / 2)) * -1
    distance11 = adsk.fusion.DistanceExtentDefinition.create(
        adsk.core.ValueInput.createByReal((grooveCenter + .05) * -1))
    distance11A = adsk.fusion.DistanceExtentDefinition.create(
        adsk.core.ValueInput.createByReal(grooveCenter - .05))
    deg0 = adsk.core.ValueInput.createByString("0 deg")
    stemGrooveExtInput.setTwoSidesExtent(distance11, distance11A, deg0, deg0)
    stemGrooveExtInput.participantBodies = [stemExt.bodies.item(0)]
    stemGrooveExt = extrudes.add(stemGrooveExtInput)
    # Change to inches in Parameters
    extent_11A = stemGrooveExt.extentOne
    extent_11B = stemGrooveExt.extentTwo
    distanceMP_11A = extent_11A.distance
    distanceMP_11B = extent_11B.distance
    distanceMP_11A.expression = "{:.{}f}".format((((grooveCenter + .05) * -1) / sizeUnits), 4) + 'in'
    distanceMP_11B.expression = "{:.{}f}".format(((grooveCenter + .05) / sizeUnits), 4) + 'in'
    stemGrooveExt.name = 'Stem Groove'

    # Create body with combine
    plugBody = plugExt.bodies[0]
    bodyCollection = adsk.core.ObjectCollection.create()
    bodyCollection.add(plugStraightExt.bodies[0])
    bodyCollection.add(hexExt.bodies[0])
    bodyCollection.add(stemExt.bodies[0])
    model = design.activeComponent
    features = model.features
    combineFeat = features.combineFeatures
    combineInput = combineFeat.createInput(plugBody, bodyCollection)
    combineFeatur = combineFeat.add(combineInput)

    # Create the chamfer
    edgeCol = adsk.core.ObjectCollection.create()
    edgeCol.clear()
    edges = stemExt.sideFaces.item(0).edges
    for edgeI in edges:
        edgeCol.add(edgeI)

    chamferFeats = newComp.features.chamferFeatures
    chamferInput = chamferFeats.createInput(edgeCol, True)
    chamferInput.setToEqualDistance(
        adsk.core.ValueInput.createByReal((numStemDiam - numHoleThru)/4))
    chamferFeats.add(chamferInput)

[BrianEkins]

This is still missing information needed to construct the model. Either an existing f3d or a full program will be best.

[Jorge_Jaramillo · Accepted solution]

@Jorge_Jaramillo - this post is being edited to remove PII.

Hi,

I believe your problem is after your combine the bodies into a single one under plugBody in this section:

Once you combine the bodies, including there the body that produced the stemExt feature, the stemExt doesn't contain side faces anymore because they become BRebFaces on the new body.

So, I think you have two options:

1. Make the chamfer before the combine feature, or

2. Look for the edges in the combined body to make the chamfer.

I hope this could solve your problem.

Best regards,

Jorge Jaramillo

[brad.bylls · Accepted solution]

I moved it up before the combined feature and now it works great.
Thanks.

[brad.bylls]

Moved it up before the combined feature and it works great.
Thanks.