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
Try
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()
objColl.Add(p)
End If
End If
Next
Catch ex As Exception
MsgBox("Exception was thrown while searching for faces")
Return
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)
Try
' 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")
Try
Dim wp1 As WorkPlane = createWorkplane(oTg.CreatePoint(0, 0, 0), oTg.CreatePoint(1, 0, 0), oTg.CreatePoint(0, 1, 0))
drawLogo(doc, wp1)
createLoft()
view.Fit()
addLogoText(wp1)
view.Fit()
wishText(wp1)
view.Fit()
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
camera.Apply()
view.Fit()
Catch ex As Exception
MsgBox(ex.Message)
Finally
trans.End()
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
extrudeText(sketch)
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)
extrudeText(sketch)
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)
Try
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))
lineTo(startPoint)
view.Fit()
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)
lineTo(startPoint)
view.Fit()
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)
Catch
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
Else
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:
Clint Brown 
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