Best Wishes & A Loft Feature

By Jelte de Jong

I wish you all the best for 2021. I hope that we can go back to normal life this year. Today I have a iLogic rule for you that creates an “I” similar to the image above. 

Nothing that you can’t find anywhere else on the internet. Just some profiles on a sketch that are extruded. Except for the loft in the Inventor logo. While I was creating this model, I discovered that you will find examples for creating loft features. I found posts with examples for creating lofts that uses rail. But none examples for using transitions.

Of course, I would like to use those transitions. After some digging around, I found how to do it. All the transitions are saved in a “MapPointCurves” object that you need to create. Default this object is not set in the “LoftDefinition” object. That made it hard to find and edit the transitions.

The first function in the iLogic rule below shows how to create the loft with transitions.

Here’s the iLogic code:

Public Class ThisRule

    Private Sub createLoft()
        ' find 2 faces for the loft
        Dim objColl As ObjectCollection
			objColl = ThisApplication.TransientObjects.CreateObjectCollection()
	        For Each face As Face In def.SurfaceBodies.Item(1).Faces
	            If (Face.GeometryForm = 9) Then
	                If (DoubleForEquals.IsEqual( Face.Evaluator.Area, 100)) Then

	                    Dim s As PlanarSketch = def.Sketches.Add(Face, True)
	                    Dim p As Profile = s.Profiles.AddForSolid()
	                End If
	            End If
		Catch ex As Exception
			MsgBox("Exception was thrown while searching for faces")
		End Try
		If (objColl.Count <> 2) Then
			Throw New Exception("Did not find the 2 faces for creating the Loft")
		End If
		' create a LoftDefinition object
	    Dim loftDef As LoftDefinition = def.Features.LoftFeatures.CreateLoftDefinition(objColl, PartFeatureOperationEnum.kJoinOperation)

	        ' create an object for the mapping of the points
	        Dim curves As MapPointCurves = def.Features.LoftFeatures.CreateMapCurves(objColl)

	        ' create a curve and and give posistion of start and end point
	        Dim curve1 = curves.AddMapCurve()
	        curve1.SetPositionUsingPoint(2, oTg.CreatePoint(0, 0, 0))
	        curve1.SetPositionUsingPoint(1, oTg.CreatePoint(10, 20, 0))

	        Dim curve2 = curves.AddMapCurve()
	        curve2.SetPositionUsingPoint(2, oTg.CreatePoint(10, 0, 0))
	        curve2.SetPositionUsingPoint(1, oTg.CreatePoint(10, 20, -10))

	        Dim curve3 = curves.AddMapCurve()
	        curve3.SetPositionUsingPoint(2, oTg.CreatePoint(10, 0, -10))
	        curve3.SetPositionUsingPoint(1, oTg.CreatePoint(0, 20, -10))

	        Dim curve4 = curves.AddMapCurve()
	        curve4.SetPositionUsingPoint(2, oTg.CreatePoint(0, 0, -10))
	        curve4.SetPositionUsingPoint(1, oTg.CreatePoint(0, 20, 0))

	        loftDef.MapPointCurves = curves
		Catch ex As Exception
			MsgBox("Unable to create transitions")
		End Try
        Dim loftFeature As LoftFeature = def.Features.LoftFeatures.Add(loftDef)
    End Sub

    Private lastPoint2D As SketchPoint
    Private currentSketch As PlanarSketch
    Private oTg As TransientGeometry
    Private def As PartComponentDefinition
    Private doc As PartDocument
    Private view As Inventor.View

    Sub Main()

        oTg = ThisApplication.TransientGeometry
        doc = ThisApplication.Documents.Add(DocumentTypeEnum.kPartDocumentObject)
        def = doc.ComponentDefinition
        view = ThisApplication.ActiveView

        Dim oAssets As Assets = doc.Assets
        Dim assetOrrange As Asset = doc.ActiveAppearance
        Dim generic_color As ColorAssetValue = assetOrrange.Item("generic_diffuse")
        generic_color.Value = ThisApplication.TransientObjects.CreateColor(236, 164, 74)
        generic_color.HasConnectedTexture = True

        Dim trans As Transaction = ThisApplication.TransactionManager.StartTransaction(doc, "create")

            Dim wp1 As WorkPlane = createWorkplane(oTg.CreatePoint(0, 0, 0), oTg.CreatePoint(1, 0, 0), oTg.CreatePoint(0, 1, 0))
            drawLogo(doc, wp1)

            Dim camera As Camera = ThisApplication.ActiveView.Camera
            camera.Perspective = True
            camera.Eye = oTg.CreatePoint(-8.9, 90.7, 169.9)
            camera.Target = oTg.CreatePoint(39.2, -3.7, -5)
            camera.UpVector = oTg.CreateUnitVector(0.126, 0.887, -0.444)
            camera.Animating = True


        Catch ex As Exception

        End Try

    End Sub
    Private Sub wishText(WorkPlane As WorkPlane)
        Dim sketch As PlanarSketch = def.Sketches.Add(WorkPlane)

        Dim text As String = "<StyleOverride FontSize='6'>We wish you the best for</StyleOverride><Br/><StyleOverride FontSize='11,'>2021</StyleOverride>"
        Dim textBox As Inventor.TextBox = sketch.TextBoxes.AddFitted(oTg.CreatePoint2d(39, -10), text)
        textBox.HorizontalJustification = HorizontalTextAlignmentEnum.kAlignTextCenter

    End Sub

    Private Sub addLogoText(workPlane As WorkPlane)
        Dim sketch As PlanarSketch = def.Sketches.Add(workPlane)
        Dim text As String = "<StyleOverride FontSize='11,'>Unofficial</StyleOverride><Br/><StyleOverride FontSize='11,'>Inventor</StyleOverride>"

        sketch.TextBoxes.AddFitted(oTg.CreatePoint2d(18, 26), text)

    End Sub

    Private Sub extrudeText(sketch As PlanarSketch)
        Dim oProfile As Profile = sketch.Profiles.AddForSolid()
        Dim oExtrudeDef As ExtrudeDefinition = def.Features.ExtrudeFeatures.CreateExtrudeDefinition(oProfile, PartFeatureOperationEnum.kJoinOperation)
        oExtrudeDef.SetDistanceExtent(1, PartFeatureExtentDirectionEnum.kNegativeExtentDirection)
        Dim oExtrude As ExtrudeFeature = def.Features.ExtrudeFeatures.Add(oExtrudeDef)
    End Sub

    Private Function createWorkplane(point1 As Point, point2 As Point, point3 As Point)
        Dim p1 = def.WorkPoints.AddFixed(point1)
        Dim p2 = def.WorkPoints.AddFixed(point2)
        Dim p3 = def.WorkPoints.AddFixed(point3)
        Dim wp As WorkPlane = def.WorkPlanes.AddByThreePoints(p1, p2, p3)
        p1.Visible = False
        p2.Visible = False
        p3.Visible = False
        wp.Visible = False
        Return wp
    End Function

    Private Sub drawLogo(doc As PartDocument, wp1 As WorkPlane)
	        currentSketch = def.Sketches.Add(wp1)
	        lastPoint2D = currentSketch.SketchPoints.Add(oTg.CreatePoint2d(0, 0))
	        Dim startPoint As SketchPoint = lastPoint2D

	        Dim ls = arcTo(oTg.CreatePoint2d(-2, 0), oTg.CreatePoint2d(-2, -2))
	        lineTo(oTg.CreatePoint2d(-5, -2))
	        lineTo(oTg.CreatePoint2d(-5, -6))
	        arcTo(oTg.CreatePoint2d(5, -86), oTg.CreatePoint2d(15, -6))
	        lineTo(oTg.CreatePoint2d(15, -2))
	        lineTo(oTg.CreatePoint2d(12, -2))
	        arcTo(oTg.CreatePoint2d(12, 0), oTg.CreatePoint2d(10, 0))

	        lastPoint2D = currentSketch.SketchPoints.Add(oTg.CreatePoint2d(0, 20))
	        startPoint = lastPoint2D
	        arcTo(oTg.CreatePoint2d(-2, 20), oTg.CreatePoint2d(-2, 22), True)
	        lineTo(oTg.CreatePoint2d(-5, 22))
	        lineTo(oTg.CreatePoint2d(-5, 26))
	        arcTo(oTg.CreatePoint2d(5, 106), oTg.CreatePoint2d(15, 26), True)
	        lineTo(oTg.CreatePoint2d(15, 22))
	        lineTo(oTg.CreatePoint2d(12, 22))
	        arcTo(oTg.CreatePoint2d(12, 20), oTg.CreatePoint2d(10, 20), True)

	        Dim oProfile As Profile = currentSketch.Profiles.AddForSolid()
	        Dim oExtrudeDef As ExtrudeDefinition = def.Features.ExtrudeFeatures.CreateExtrudeDefinition(oProfile, PartFeatureOperationEnum.kJoinOperation)
	        Call oExtrudeDef.SetDistanceExtent(10, PartFeatureExtentDirectionEnum.kNegativeExtentDirection)
	        Dim oExtrude As ExtrudeFeature = def.Features.ExtrudeFeatures.Add(oExtrudeDef)
			MsgBox("Exception was thrown while creating logo")
		End Try
    End Sub

    Private Function arcTo(centerPoint As Point2d, EndPoint As Point2d, Optional CounterClockwise As Boolean = False)
        Dim l = currentSketch.SketchArcs.AddByCenterStartEndPoint(centerPoint, lastPoint2D, EndPoint, CounterClockwise)
        If (CounterClockwise) Then
            lastPoint2D = l.EndSketchPoint
            lastPoint2D = l.StartSketchPoint
        End If
        Return l
    End Function
    Private Function lineTo(EndPoint)
        Dim l As SketchLine = currentSketch.SketchLines.AddByTwoPoints(lastPoint2D, EndPoint)
        lastPoint2D = l.EndSketchPoint
        Return l
    End Function

End Class

About the Author:

Jelte de Jong works for a company that creates custom heat exchangers. He has used Inventor for over 10 years. Jelte has worked mostly as a mechanical engineer, but in recent years he has combined his hobby (programming) with his professional life. He now works as a software/mechanical engineer. His main task is supporting the drawing office by creating and maintaining configurable models and Inventor add-ins.

Find Jelte de Jong here:

Blog | Autodesk Forum | LinkedIn | Autodesk App Store

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