Model parameters, expressions and values.

[brad.bylls]

Using the below code to create an extrusion.

I am able to change the top name(yellow) of the parameter.

What I would like to do is change the sub-name(blue) and the 'Name'(green)

Lastly I would like to change the expression(red) to be the same as the value(in)

Because it is a TwoSidesExtent, I am at a loss as to how to do it.

# Create the head clearance

        cutHeadSketch = sketches.add(xyPlane)

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

        distance1 = adsk.fusion.DistanceExtentDefinition.create(adsk.core.ValueInput.createByReal(numBoltClearanceLength - numBoltBodyLength))

        distance2 = adsk.fusion.DistanceExtentDefinition.create(adsk.core.ValueInput.createByReal(numBoltTravelLength))

        deg0 = adsk.core.ValueInput.createByString("0 deg")

        cutHeadExtInput.setTwoSidesExtent(distance1, distance2, deg0, deg0)

        cutHeadExt = extrudes.add(cutHeadExtInput)

        cutHeadExt.name = 'Head Clearance Extrude'

[kandennti · Accepted solution]

Hi @brad.bylls .

I don't think sub-name (blue) can be changed.
(I couldn't do it even with GUI)

'Name' (green) can be changed by getting the model parameters.

https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-86e451c2-785f-4cdf-97c9-ecba4882c8d1 

Wouldn't expression (red) be'in'by using createByString?

        # Head Clearance Sketch
        cutHeadSketch = sketches.add(xyPlane)
        cutHeadSketch.name = 'Head Clearance Sketch'

        cutHeadCircle = cutHeadSketch.sketchCurves.sketchCircles.addByCenterRadius(center, numBoltCboreDiam/2)
        cutHeadCircle_Dia = cutHeadSketch.sketchDimensions.addDiameterDimension(cutHeadCircle, adsk.core.Point3D.create(-1, 1, 0))
        cutHeadCircle_Dia.parameter.name = 'BoltCboreDiam'# parameter rename
        
        # Head Clearance Extrude
        cutHeadProf = cutHeadSketch.profiles[0]
        cutHeadExtInput = extrudes.createInput(cutHeadProf, adsk.fusion.FeatureOperations.NewBodyFeatureOperation)

        distance1 = adsk.fusion.DistanceExtentDefinition.create(
            adsk.core.ValueInput.createByString('{} in'.format(numBoltClearanceLength - numBoltBodyLength)))# use createByString

        distance2 = adsk.fusion.DistanceExtentDefinition.create(
            adsk.core.ValueInput.createByString('{} in'.format(numBoltTravelLength)))# use createByString

        deg0 = adsk.core.ValueInput.createByString("0 deg")

        cutHeadExtInput.setTwoSidesExtent(distance1, distance2, deg0, deg0)
        cutHeadExt = extrudes.add(cutHeadExtInput)
        cutHeadExt.name = 'Head Clearance Extrude'

        cutHeadExt.extentOne.distance.name = 'Head_Length'# parameter rename
        cutHeadExt.extentTwo.distance.name = 'Travel_Length'# parameter rename
        cutHeadExt.taperAngleOne.name = 'Head_Angle'# parameter rename
        cutHeadExt.taperAngleTwo.name = 'Travel_Angle'# parameter rename

[brad.bylls]

Thank you for the help.

It worked.