Manufacturing DevBlog

Number of items in a circular pattern feature

By Augusto Goncalves

The number of items in circular pattern feature are stored as model parameters. The Count method of CircularPatternFeature has a property value, setting this value actually modifies the corresponding model feature.

Public Sub ChangeNumberOfFeatures()

  ' check if the document is a Part Document

  If m_inventorApplication.ActiveDocumentType _

    <> DocumentTypeEnum.kPartDocumentObject Then Exit Sub

 

  Dim part As PartDocument = _

    m_inventorApplication.ActiveDocument

 

  Try

    ' Change the number of features in the pattern.

    part.ComponentDefinition.Features. _

      CircularPatternFeatures(1).Count.Value = 8

 

    ' update Inventor

    m_inventorApplication.ActiveDocument.Update()

 

  Catch ex As SystemException

    ' Add a Circular Pattern Feature

  End Try

End Sub

Introducing ADN Open

By Stephen Preston

(Cross posted across all ADN DevBlogs)

Those of you who have been watching carefully will have noticed that the ADN DevTech team has been doing a few things differently recently:

• We’ve launched these DevBlogs , and have been steadily moving technical content (a.k.a. DevNotes) from the members-only ADN website to here, along with posting new content.
• We’ve been increasing our presence in the Autodesk discussion groups that cover our product APIs.
• We’ve revamped our Developer Centers to update and (hopefully) more clearly document the resources available to developers who want to use Autodesk technology as part of their software solutions. That includes our recent ‘My First Plug-in’ tutorials for AutoCAD, Revit and Inventor.

This is all part of our master plan to hold the world to ransom for ONE MILLION DOLLARS! …

Oops – hang on – that was my other plan. Try again …

This is all part of our plan to make information on Autodesk technology more accessible to people who can’t afford the fee for full ADN membership, and/or who are evaluating the best technology to use to implement a new solution and want to be able to quickly find the best tools for the job via a simple web search. All of these changes have been our putting the pieces in place so that we can formally announce ADN Open.

So that’s the basics. You can quickly browse www.autodesk.com/adnopen and stop reading here if you like. But if you want more information, read on (if you’re an ADN Standard or ADN Professional member, you should have received similar information on this via the ADN DevNews newsletter) …

 

What is Changing?

Along with the two existing types of ADN membership – Standard and Professional – we now have ADN Open .  ADN Open consists of software developer focused blogs, moderated discussion groups (forums), training materials, and more - that are available to everyone and anyone for free. The two most noteworthy changes are:

 

We are migrating all non-confidential software development information previously available through the password protected ADN website to ADN Open DevBlogs.

This means that a simple Google search – something most of you already do to look for solutions to your problems - will now include crawling the thousands of DevNotes that Autodesk DevTech engineers have published.  We believe this change will result in your getting better answers to your problems faster, using the same search technology you already use every day.

We expect to complete this migration task within the next few months, and we’re posting new information to the blogs at the same time.

 

Participation in the Autodesk public API discussion groups (forums) will increase.

We will be offering ADN Standard and Professional members the option to either ask their question in private (as they have always done), or to ask their questions on the forums. The DevTech team will be monitoring the forums to ensure that these questions are answered. While we’re there, we’ll also help out with other questions. We anticipate that our involvement, and the increased involvement from ADN members who previously asked questions in private, will further enhance these already thriving communities.

Check out the ADN Open web site – www.autodesk.com/adnopen - for a current list of Autodesk technology now being actively supported through public DevBlogs and API discussion groups.

If you’re an ADN Standard or Professional member, please read your ADN DevNews newsletter for more information on this.

 

Why do we still offer Standard and Professional ADN membership?

There are additional benefits to ADN Standard and Professional membership.  You’ll want to maintain your ADN Standard or Professional membership if you:

• Need access to Autodesk desktop products – easy download and perpetual license through the ADN extranet
• Access to Autodesk beta software.
• Want an Autodesk engineer to help you with a confidential issue/question.
• Need API support for the few Autodesk technologies not supported through ADN Open – only the forums listed on www.autodesk.com/adnopen will be supported by the DevTech team.
• Want your product, services and company information visible to hundreds of thousands of Autodesk customers on www.autodesk.com/partnerproducts.

Please visit www.autodesk.com/joinadn if you’re interested in upgrading from ADN Open to ADN Standard or Professional to take advantage of these additional benefits.

 

Why the Change?

The Autodesk Developer Network was designed during a time of a rapidly expanding market for desktop design, engineering and entertainment software.  This was a time of growing sales of heavy desktop software, never enough computing power, and limited connectivity.  The investment to start and grow a software company was significant.    

The software industry is now undergoing a period of rapid change and innovation driven by cloud enabled, limitless, low cost computing power; rapidly expanding near ubiquitous connectivity through the internet and mobile devices and cross-platform support for key web technologies including HTML5 and Java.  Cloud and mobile technologies - along with the increasingly social behavior of software entrepreneurs and programmers - is changing the software industry, our personal and business lives, and the world we live in.

By modernizing the ADN program to better fit with these technology driven changes, we believe we can significantly improve the service we provide to software developers who choose ADN Professional or Standard membership levels, provide much better assistance to software developers who don’t need the additional ADN benefits, and make it easier for a new generation of innovators to discover and evaluate our technology.

 

Questions?

If you have any questions about this, then you’re welcome to comment on this blog post or email me directly.

Change the Browser Node icon

By Augusto Goncalves

To change the icon on the existing Browser Node, you need to create a standard Microsoft Windows IPictureDisp referencing an image(.bmp/.gif/.jpg) file, then add the IPictureDisp to the client node resource and apply this new client node resource to Client Browser Node Definition object.

The following sample code requires reference to stdole type library and Microsoft.VisualBasic.Compatibility assembly.

Sub modifyIcon()

  Dim oDoc As Inventor.Document

  oDoc = m_inventorApplication.ActiveDocument

 

  ' Find the specified Browser Pane

  Dim oPane As Inventor.BrowserPane

  oPane = oDoc.BrowserPanes.Item("NewPane")

 

  Dim oNode As BrowserNode

  oNode = oPane.TopNode

 

  Dim oDef As ClientBrowserNodeDefinition

  oDef = oNode.BrowserNodeDefinition

 

  ' Create a standard Microsoft Windows IPictureDisp

  ' load image

  Dim bmp As System.Drawing.Bitmap = _

    New System.Drawing.Bitmap("c:\temp\a.bmp")

  Dim resourcePic As IPictureDisp

  resourcePic = Microsoft.VisualBasic. _

    Compatibility.VB6.ImageToIPictureDisp(bmp)

  ' Create new Client Node Resource

  Dim oRsc As Inventor.ClientNodeResource

  oRsc = oDoc.BrowserPanes.ClientNodeResources. _

    Add("MyRsc", 2, resourcePic)

 

  ' Change the icon

  oDef.Icon = oRsc

End Sub

Get ComponentDefinition of suppressed component in BOM

By Xiaodong Liang

Issue
My code accesses BOM of the assembly and check the ComponentDefinition of each BOM row. It works well with the  Master view, but in an LOD view, it failed to check the BOM row whose component is suppressed .

Solution
The suppressed component will not have the ComponentDefinitions value on the BOMRow object. This is as designed. The statement in Inventor API document says:
Suppression
An instance in an assembly can now be suppressed for capacity gains. This means that the connection to the referenced document from the particular instance is ignored, and the referenced document is available to be closed if otherwise unreferenced. Any APIs that traverse across that instance to the referenced document will not be able to succeed. This would include operations on ComponentOccurrence such as the Definition, SubOccurrences, and SurfaceBodies properties. Binding reference keys or obtaining the attached entities of an Attribute that reside across the suppressed connection will likewise be impossible to satisfy.
A suppressed link will behave much as an unresolved link did in previous releases. An application would usually want to treat a suppressed connection much as they would have treated an unresolved reference in previous releases. The issue is that many applications likely did not pay much attention to unresolved dependency situations, but now with suppression it will be much more common, and may occur during the working lifetime of the referencing document instead of only at open time.

The workaround is to obtain the BOMRow.ReferencedFileDescriptor.ReferencedFile.AvailableDocuments(1).ComponentDefinition instead when failing to get the ComponentDefinitions from the BOMRow object.

Extrude the Text in Inventor

By Augusto Goncalves

Inventor supports the extrusion of Text object. The following sample code demonstrates how to extrude the text.

Public Sub ExtrudeText()

  'create a part Document

  Dim oPartDoc As PartDocument

  oPartDoc = m_inventorApplication.Documents.Add( _

    DocumentTypeEnum.kPartDocumentObject, _

    m_inventorApplication.FileManager.GetTemplateFile( _

      DocumentTypeEnum.kPartDocumentObject))

 

  Dim oCompDef As PartComponentDefinition

  oCompDef = oPartDoc.ComponentDefinition

 

  'get the xy work plane

  Dim oSketch As PlanarSketch

  oSketch = oCompDef.Sketches.Add( _

    oCompDef.WorkPlanes.Item(3))

 

  ' access the transient geometry object

  Dim oTG As TransientGeometry

  oTG = m_inventorApplication.TransientGeometry

 

  Call oSketch.SketchLines.AddAsTwoPointRectangle( _

    oTG.CreatePoint2d(0, 0), oTG.CreatePoint2d(20, 10))

 

  ' prepare the skecth for extrusion

  Dim oProfile As Profile

  oProfile = oSketch.Profiles.AddForSolid

 

  ' create the extrusion

  Dim oExtrudeDef As ExtrudeDefinition = _

    oCompDef.Features.ExtrudeFeatures. _

    CreateExtrudeDefinition(oProfile, _

      PartFeatureOperationEnum.kJoinOperation)

  oExtrudeDef.SetDistanceExtent(2, _

      PartFeatureExtentDirectionEnum.kNegativeExtentDirection)

  Dim oExtrude As ExtrudeFeature

  oExtrude = oCompDef.Features.ExtrudeFeatures.Add(oExtrudeDef)

 

  ' get the active camera and fit the view

  Dim oCamera As Camera

  oCamera = m_inventorApplication.ActiveView.Camera

  oCamera.ViewOrientationType = ViewOrientationTypeEnum. _

    kIsoTopLeftViewOrientation

  oCamera.Fit()

  oCamera.Apply()

 

  'Place Sketch Text  

  oSketch = oCompDef.Sketches.Add( _

    oExtrude.StartFaces.Item(1))

  Dim oText As TextBox

  oText = oSketch.TextBoxes.AddByRectangle( _

    oTG.CreatePoint2d(0, 0), _

    oTG.CreatePoint2d(20, 10), _

    "<StyleOverride FontSize='2.54' Bold='True'>" +

    "Sample</StyleOverride>")

  oText.HorizontalJustification = _

    HorizontalTextAlignmentEnum.kAlignTextCenter

  oText.VerticalJustification = _

    VerticalTextAlignmentEnum.kAlignTextMiddle

 

  'Extrude Text 

  oProfile = oSketch.Profiles.AddForSolid

  oExtrude = oCompDef.Features.ExtrudeFeatures. _

    AddByDistanceExtent(oProfile, 0.5, _

          PartFeatureExtentDirectionEnum. _

          kPositiveExtentDirection, _

          PartFeatureOperationEnum.kJoinOperation)

End Sub

Normal Vectors and Points on BREP surfaces

By Augusto Goncalves

(1) Does the Normal Vector returned by Face.Evaluator.GetNormal() point into, or out of the material in a solid?

When used on a solid - Face.Evaluator.GetNormal() returns normal vectors pointing away from the solid material, into void. The same is true of FaceProxy.Evaluator.GetNormal()

(2) What does Face.IsParamReversed = True mean?

Geometry obtained from BRep entity maybe aligned or opposed with this BRep entity, IsParamReversed property indicates whether the underlying geometry is consistent or reversed with the BRep. So if you use Face.Geometry.Evaluator.GetNormal(), and Face.IsParamReversed is true, then the normals returned only need to be reversed to point out of the solid.

(3) Do calls return the same value, and does Face.IsParamReversed affect the result?
Face.Evaluator.GetPointAtParam(u, v)
Face.Geometry.Evaluator.GetPointAtParam(u, v);

Face.Evaluator.GetPointAtParam() and Face.Geometry.Evaluator.GetPointAtParam() return a same point for a given u,v coordinate.The same is also true when considering FaceProxy objects. Face.IsParamReversed do affect on the result.

What is the Best Way to Compute a Normal of a Face in Inventor API?

By Barbara Han

There can be many ways to compute a face's normal using the geometric information provided by the Inventor objects. However, the best way to compute a normal using the API is to use the Face.Evaluator object.

Here is a sample that iteratesthroughl faces of a SurfaceBody and output the normal vectors for the faces that are planar.

VBA sample:

Public Sub ComputePlanarFacesNormals()

 

    Dim oPartDoc As PartDocument

    Set oPartDoc = ThisApplication.ActiveDocument

   

    Dim oFaces As Faces

    Set oFaces = oPartDoc.ComponentDefinition.SurfaceBodies(1).Faces

   

    Dim Params(1 To 2) As Double

    Dim Normals(1 To 3) As Double

   

    'If Faces is planar, then the Normal wil be the same all over the face

    Params(1) = 0

    Params(2) = 0

   

    Dim index As Long

    index = 1

   

    Dim oFace As Face

    For Each oFace In oFaces

   

        'Ensures Face is planar

        If (TypeOf oFace.Geometry Is Plane) Then

   

            Call oFace.Evaluator.GetNormal(Params, Normals)

           

            Dim oUnitNormal As UnitVector

            Set oUnitNormal = ThisApplication.TransientGeometry.CreateUnitVector(Normals(1), Normals(2), Normals(3))

           

            Debug.Print "Planar Face[" & index & "] Normal: [" & oUnitNormal.X & ", " & oUnitNormal.Y & ", " & oUnitNormal.Z & "]"

           

            index = index + 1

           

        End If

   

    Next

 

End Sub

VB.NET sample:

Private SubComputePlanarFacesNormals()

    Try

 

        Dim oPartDoc As PartDocument = m_inventorApp.ActiveDocument

 

        Dim oFaces As Faces

        oFaces = oPartDoc.ComponentDefinition.SurfaceBodies(1).Faces

 

        Dim Params(0 To 3) As Double

        Dim Normals(0 To 3) As Double

 

        'If Faces is planar, then the Normal wil be the same all over the face

        Params(1) = 0

        Params(2) = 0

 

        Dim index As Long = 1

 

        Dim oFace As Face

        For Each oFace In oFaces

 

            'Ensures Face is planar

            If (TypeOf oFace.Geometry Is Plane) Then

 

                Call oFace.Evaluator.GetNormal(Params, Normals)

 

                Dim oUnitNormal As UnitVector

                oUnitNormal = m_inventorApp.TransientGeometry.CreateUnitVector(Normals(1), Normals(2), Normals(3))

 

                System.Diagnostics.Debug.Write("Planar Face[" & index & "] Normal: [" & oUnitNormal.X & ", " & oUnitNormal.Y & ", " & oUnitNormal.Z & "]" & vbCrLf)

 

                index = index + 1

 

            End If 

        Next

    Catch ex As Exception

        MsgBox(ex.ToString())

    End Try

End Sub

Use XDirectionMidPlanePattern and YDirectionMidPlanePattern for symmetrical Rectangular pattern

By Wayne Brill

Issue

I am trying to use the API to create a Rectangular Pattern that is symmetrical around the feature being used for the pattern. I am not finding a way to use the parameters of the RectangularPatternFeatures.Add method to achieve the same results that I get using the MidPlane option in the UI. Is there a way to achieve this using the API?

Solution

The API does not provide the MidPlane option on forward create. But you can edit the feature to get the desired result. Here are a VBA and VB.NET examples that shows how this can be done. Before running have an extrusion with a hole that can be used for the pattern. (have the hole near the middle of the face)

VBA

Sub PatternRectTest()

    Dim oDoc As PartDocument
    Set oDoc = ThisApplication.ActiveDocument
   
    Dim oCompDef As PartComponentDefinition
    Set oCompDef = oDoc.ComponentDefinition
   
    Dim objColFeatures As ObjectCollection
    Set objColFeatures = ThisApplication. _
    TransientObjects.CreateObjectCollection
   
    Call objColFeatures.Add _
    (oCompDef.Features.HoleFeatures.Item(1))
   
    Dim oRectFeature As RectangularPatternFeature
    Set oRectFeature = oCompDef.Features. _
    RectangularPatternFeatures.Add(objColFeatures, _
    oCompDef.WorkAxes.Item _
    ("X Axis"), False, 3, "1 in", , , _
    oCompDef.WorkAxes.Item _
    ("Y Axis"), True, 3, "1 in", , , kOptimizedCompute)
   
    oRectFeature.XDirectionMidPlanePattern = True
    oRectFeature.YDirectionMidPlanePattern = True
   
End Sub

VB.NET

Public Class Form1

 

    Dim m_inventorApp As Inventor.Application _

                                       = Nothing

 

    Private Sub Button1_Click(ByVal sender As  _

                                System.Object, _

                  ByVal e As System.EventArgs) _

                        Handles Button1.Click

 

        ' Get an active instance of Inventor

        Try

            m_inventorApp = System.Runtime. _

                   InteropServices.Marshal. _

       GetActiveObject("Inventor.Application")

          

        Catch 'Inventor not started

            System.Windows.Forms.MessageBox. _

             Show("Start an Inventor session")

            Exit Sub

        End Try

 

        'Call the Sub

        test()

    End Sub

 

    Sub test()

        Dim oDoc As PartDocument = _

                   m_inventorApp.ActiveDocument

 

        Dim oCompDef As PartComponentDefinition = _

                            oDoc.ComponentDefinition

 

        Dim objColFeatures As ObjectCollection = _

m_inventorApp.TransientObjects.CreateObjectCollection

 

        Call objColFeatures.Add _

             (oCompDef.Features.HoleFeatures.Item(1))

 

        Dim oRectFeature As RectangularPatternFeature

        oRectFeature = oCompDef.Features. _

     RectangularPatternFeatures.Add(objColFeatures, _

        oCompDef.WorkAxes.Item _

        ("X Axis"), False, 3, "1 in", , , _

        oCompDef.WorkAxes.Item("Y Axis"), _

        True, 3, "1 in", , , _

        PatternComputeTypeEnum.kOptimizedCompute)

 

        oRectFeature.XDirectionMidPlanePattern = True

        oRectFeature.YDirectionMidPlanePattern = True

    End Sub

 

End Class

Transparency of ClientGraphics - when RenderStyle is set makes a difference in 2012

By Wayne Brill

Issue

I need to create ClientGraphics that are transparent. I use the RenderStyle property of a ClientNode and set it to a render style that is transparent. In Inventor 2012 my ClientGraphics are not transparent. The same code running in Inventor 2011 was transparent. Is there a way to get the ClientGraphics to be transparent in 2012?

Solution

The solution in the 2012 release is to call RenderStyle soon after the ClientNode is created. This VBA example that is an update from the help file will help explain. Notice that RenderStyle() for the GraphicsNode is called right after it is created.

Note: Behavior does not occur in Inventor 2013.

Public Sub DrawCustomTriangles()
    Dim oDoc As Document
    Set oDoc = ThisApplication.ActiveDocument

    ' Set a reference to component definition of
    ' the active document. This assumes that a part
    ' or assembly document is active.
    Dim oCompDef As ComponentDefinition
    Set oCompDef = ThisApplication.ActiveDocument _ 
                             .ComponentDefinition
   
    ' Check to see if the test graphics data object
    ' already exists. If it does clean up by removing
    ' all associated of the client graphics from the
    'document. If it doesn't create it and draw a line.
    On Error Resume Next
    Dim oGraphicsData As GraphicsDataSets
    Set oGraphicsData = oDoc.GraphicsDataSetsCollection _ 
                               .Item ("SampleGraphicsID")
    If Err.Number = 0 Then
        On Error GoTo 0
       ' An existing client graphics object was
        'successfully obtained so clean up.
        oGraphicsData.Delete
        oCompDef.ClientGraphicsCollection.Item _
                            ("SampleGraphicsID").Delete
   
        ' update the display to see the results.
        ThisApplication.ActiveView.Update
    Else
        Err.Clear
        On Error GoTo 0
       
       ' Set a reference to the transient geometry
        ' object for user later.
        Dim oTransGeom As TransientGeometry
        Set oTransGeom = ThisApplication.TransientGeometry
       
        ' Create a graphics data set object.  This object
        ' contains all of the
        ' information used to define the graphics.
        Dim oDataSets As GraphicsDataSets
        Set oDataSets = oDoc.GraphicsDataSetsCollection _
                                  .Add ("SampleGraphicsID")
       
        ' Create a coordinate set.
        Dim oCoordSet As GraphicsCoordinateSet
        Set oCoordSet = oDataSets.CreateCoordinateSet(1)

        ' Get the number of sides for the cylinder.
        Dim iSideCount As Long
        iSideCount = InputBox _
("Enter number of sides for cylinder.(Must be greater than 2.)", _
                                  "Cylinder Tolerance", 25)
       
        Dim dRadius As Double
        Dim dHeight As Double
        dRadius = 3
        dHeight = 7
       
        ' Create an array containing points to used
        ' in drawing the cylinder. The points could also
        ' be directly defined in a coordinate set, but
        ' defining them in array and then setting the
        ' coordinates using the
        ' array is more efficient for a large set of points.
        Dim adPointCoords() As Double
        ReDim adPointCoords _
              (1 To ((iSideCount + 1) * 2) * 3) As Double
        Dim i As Long
        Dim dAngle As Double
       
        ' Define the points for the outline of
        'the first end of the cylinder.
        dAngle = 0
        For i = 0 To iSideCount - 1
            adPointCoords(i * 3 + 1) = dRadius * Cos(dAngle)
            adPointCoords(i * 3 + 2) = dRadius * Sin(dAngle)
            adPointCoords(i * 3 + 3) = 0
            ' Increment the angle for the next point
            dAngle = dAngle + _
                       ((2 * 3.14159265358979) / iSideCount)
        Next
       
        ' Define the points for the outline of the other
        ' end of the cylinder.
        dAngle = 0
        For i = iSideCount To (iSideCount * 2) - 1
            adPointCoords(i * 3 + 1) = dRadius * Cos(dAngle)
            adPointCoords(i * 3 + 2) = dRadius * Sin(dAngle)
            adPointCoords(i * 3 + 3) = dHeight
           
            ' Increment the angle for the next point
            dAngle = dAngle + _
                     ((2 * 3.14159265358979) / iSideCount)
        Next
       
        ' Define coordinate at the center of the
        'first end of the cylinder.
        adPointCoords((iSideCount * 2) * 3 + 1) = 0
        adPointCoords((iSideCount * 2) * 3 + 2) = 0
        adPointCoords((iSideCount * 2) * 3 + 3) = 0
       
        ' Define coordinate at the center of the other
        ' end of the cylinder.
        adPointCoords((iSideCount * 2) * 3 + 4) = 0
        adPointCoords((iSideCount * 2) * 3 + 5) = 0
        adPointCoords((iSideCount * 2) * 3 + 6) = dHeight

        ' Assign the points to the coordinate set.
        Call oCoordSet.PutCoordinates(adPointCoords)
       
        ' Create an index set to use for the triangle fan for
        ' cap of the first end of the cylinder.  This will
        ' serve as in index look-up into the coordinate set.
        Dim oCap1Index As GraphicsIndexSet
        Set oCap1Index = oDataSets.CreateIndexSet(1)
       
       ' Set the index values.  This could also be done
        ' by setting the value in an array and then using
        ' the array to set the values of the index set.
        ' Using an array is more efficient, but this
        ' is used to here to demonstrate the IndexSet
        ' object's Add method.
        Call oCap1Index.Add(1, iSideCount * 2 + 1)
        Call oCap1Index.Add(2, 1)
        Call oCap1Index.Add(3, 2)
        For i = 4 To iSideCount + 1
            Call oCap1Index.Add(i, i - 1)
        Next
        Call oCap1Index.Add(iSideCount + 2, 1)

        ' Create an index set to use for the
        ' triangle fan of the other cylinder cap.
        Dim oCap2Index As GraphicsIndexSet
        Set oCap2Index = oDataSets.CreateIndexSet(2)
       
        ' Set the index values.
        Call oCap2Index.Add(1, iSideCount * 2 + 2)
        Call oCap2Index.Add(2, iSideCount + 1)
        Call oCap2Index.Add(3, iSideCount + 2)
        For i = 4 To iSideCount + 1
            Call oCap2Index.Add(i, i + iSideCount - 1)
        Next
        Call oCap2Index.Add(iSideCount + 2, _
                                        iSideCount + 1)

        ' Create an index set to use for the triangle
        ' strip that will
        ' define the sides of the cylinder.
        Dim oCylinderIndex As GraphicsIndexSet
        Set oCylinderIndex = oDataSets.CreateIndexSet(3)

        ' Define the index values in an array.
        Dim iIndexValues() As Long
        ReDim iIndexValues _
                     (1 To (iSideCount + 1) * 2) As Long
        For i = 0 To iSideCount - 1
            iIndexValues(i * 2 + 1) = i + 1
            iIndexValues(i * 2 + 2) = i + iSideCount + 1
        Next
        iIndexValues(((iSideCount + 1) * 2) - 1) = 1
        iIndexValues((iSideCount + 1) * 2) = iSideCount + 1

        ' Define the index values in the index set
        ' using the array.
        Call oCylinderIndex.PutIndices(iIndexValues)

        ' Create the ClientGraphics object.
        Dim oClientGraphics As ClientGraphics
        Set oClientGraphics = oCompDef. _
          ClientGraphicsCollection.Add("SampleGraphicsID")
      
        ' Create a new graphics node within the client
        ' graphics objects.
        Dim oCylinderNode As GraphicsNode
        Set oCylinderNode = oClientGraphics.AddNode(1)
       
        'WB added
        oCylinderNode.Selectable = True
        'WB transparency works if called here
        oCylinderNode.RenderStyle = _
                   oDoc.RenderStyles.Item("Red (clear)")
       
        ' Create a triangle fan for cap 1 of the cylinder.
        Dim oCap1TriangleFan As TriangleFanGraphics
        Set oCap1TriangleFan = _
                    oCylinderNode.AddTriangleFanGraphics
        'WB it works here
        'oCylinderNode.RenderStyle = _
        'oDoc.RenderStyles.Item("Red (clear)")
      
      ' Set the coordinates and index set for the cap.
        oCap1TriangleFan.CoordinateSet = oCoordSet
        oCap1TriangleFan.CoordinateIndexSet = oCap1Index
      
        ' Create a triangle fan for cap 2 of the cylinder.
        Dim oCap2TriangleFan As TriangleFanGraphics
        Set oCap2TriangleFan = oCylinderNode. _
                                  AddTriangleFanGraphics

        ' Set the coordinates and index set for the cap.
        oCap2TriangleFan.CoordinateSet = oCoordSet
        oCap2TriangleFan.CoordinateIndexSet = oCap2Index
       
        ' WB it works here for the previously added graphics
        'oCylinderNode.RenderStyle = _
        '           oDoc.RenderStyles.Item ("Red (clear)")

        ' Create a triangle string for the sides of the cylinder.
        Dim oCylinderStrip As TriangleStripGraphics
        Set oCylinderStrip = oCylinderNode. _
                                 AddTriangleStripGraphics
        'WB does not work here
        ' oCylinderNode.RenderStyle = _
                  '  oDoc.RenderStyles.Item("Red (clear)")

        ' Set the coordinates and index set for the cap.
        oCylinderStrip.CoordinateSet = oCoordSet
        oCylinderStrip.CoordinateIndexSet = oCylinderIndex
       
       
        'oCylinderNode.RenderStyle = oDoc.RenderStyles.Item("Purple")
        'WB Added
        'WB this is not working here
      '  oCylinderNode.RenderStyle =
         'oDoc.RenderStyles.Item("Blue (clear)")
       
        ' update the display to see the results.
        ThisApplication.ActiveView.Update
 
        ' Define a normal for cap 1.
        Dim oCap1Normals As GraphicsNormalSet
        Set oCap1Normals = oDataSets.CreateNormalSet(1)
        Call oCap1Normals.Add _
              (1, oTransGeom.CreateUnitVector(0, 0, -1))
     
       ' Assign the normals to the cap.
        oCap1TriangleFan.NormalSet = oCap1Normals
       
       
        ' Define a normal for cap 2.
        Dim oCap2Normals As GraphicsNormalSet
        Set oCap2Normals = oDataSets.CreateNormalSet(2)
        Call oCap2Normals.Add _
                (1, oTransGeom.CreateUnitVector(0, 0, 1))
  
        ' Assign the normals to the cap.
        oCap2TriangleFan.NormalSet = oCap2Normals
       
        ' Create an array that contains the normals
        ' for each vertex of the cylinder.
        Dim adNormals() As Double
        ReDim adNormals _
             (1 To ((iSideCount + 1) * 2) * 3) As Double
        dAngle = 0
        For i = 0 To iSideCount
            Dim dX As Double
            Dim dY As Double
            dX = Cos(dAngle)
            dY = Sin(dAngle)
            adNormals(i * 6 + 1) = dX
            adNormals(i * 6 + 2) = dY
            adNormals(i * 6 + 3) = 0
            adNormals(i * 6 + 4) = dX
            adNormals(i * 6 + 5) = dY
            adNormals(i * 6 + 6) = 0

            ' Increment the angle for the next normal.
            dAngle = dAngle + _
                 ((2 * 3.14159265358979) / iSideCount)
        Next
       
        ' Create and set the normal set for the cylinder.
        Dim oCylinderNormals As GraphicsNormalSet
        Set oCylinderNormals = oDataSets.CreateNormalSet(3)
        Call oCylinderNormals.PutNormals(adNormals)
       
        ' Assign the normals to the cylinder.
        oCylinderStrip.NormalSet = oCylinderNormals
       
        ' Does not work here
        ' oCylinderNode.RenderStyle = _
               'oDoc.RenderStyles.Item("Blue (clear)")
       
        ' update the display to see the results.
        ThisApplication.ActiveView.Update
    End If
End Sub

Project the cutted edges of an assembly on sketch

By Augusto Goncalves

One possible solution is call programmatically the built-in command "Project Cut Edges...", which is available through the user interface.

To do it with the user interface, follow the steps:

• Select a WorkPlane in your assembly
• Using the Create Component command a part is created with a default sketch in Edit mode based on the workplane
• Select the occurrence you want to project
• Use the Project Cut Edges command

To perform the same thing programmatically, there is no direct equivalent in the API currently, however there is a workaround: this is a mix of API calls & user commands called programmatically which is following the workflow described above.

To test it, open an assembly file, select or create a workplane that intersect with the assembly and run the following sample TestProjectCutEdges method, replacing "PartTestProjection:1" by the name of the occurrence you want to project as it appears in the browser pane.

Public Sub TestProjectCutEdges()

  ' access the active document as

  ' Assembly Document

  If (m_inventorApplication.ActiveDocumentType <> _

      DocumentTypeEnum.kAssemblyDocumentObject) Then Return

  Dim oAsmDoc As AssemblyDocument

  oAsmDoc = m_inventorApplication. _

    ActiveDocument

 

  ' get the workplane

  Dim oWorkPlane As WorkPlane = TryCast(

    m_inventorApplication. _

    ActiveDocument.SelectSet.Item(1),  _

    WorkPlane)

  If (oWorkPlane Is Nothing) Then Return

 

  ' start the method

  MethodProjectCutEdges(oAsmDoc, _

                        oWorkPlane, _

                        "PartTestProjection:1")

End Sub

 

Public Sub MethodProjectCutEdges( _

                                ByVal oAsmDoc As AssemblyDocument, _

                                ByVal oWorkPlane As WorkPlane, _

                                ByVal OccurenceName As String)

  Dim xVector As Vector = Nothing

  Dim yVector As Vector = Nothing

  Dim zVector As Vector = oWorkPlane.Plane.Normal.AsVector

 

  'Create a coordinate system based on the workplane's normal vector

  CreateCoordSystem(xVector, yVector, zVector)

 

  ' create a transformation matrix

  Dim oMatrix As Matrix = m_inventorApplication. _

    TransientGeometry.CreateMatrix

  ' and set the coordinate system

  oMatrix.SetCoordinateSystem( _

    oWorkPlane.Plane.RootPoint, _

    xVector, yVector, zVector)

 

  ' create a new part document

  Dim oPartDoc As PartDocument = m_inventorApplication. _

    Documents.Add(DocumentTypeEnum.kPartDocumentObject, _

                  m_inventorApplication.FileManager. _

                  GetTemplateFile( _

                    DocumentTypeEnum.kPartDocumentObject), _

                  False)

  ' and add as an occurrence to the active assembly document

  Dim oCompOcc As ComponentOccurrence = oAsmDoc. _

    ComponentDefinition.Occurrences.AddByComponentDefinition( _

      oPartDoc.ComponentDefinition, oMatrix)

  ' and start edit mode

  oCompOcc.Edit()

 

  ' access the part document component definition

  Dim oPartCompDef As PartComponentDefinition = _

    oCompOcc.Definition

  ' and create a new sketch

  Dim oSketch As Sketch

  oSketch = oPartCompDef.Sketches.Add( _

    oPartCompDef.WorkPlanes.Item("XY Plane"))

  oSketch.Edit()

 

  ' make the part occurrence as the selection

  Dim oSelectedOcc As Object

  oSelectedOcc = oAsmDoc.ComponentDefinition. _

    Occurrences.ItemByName(OccurenceName)

  oAsmDoc.SelectSet.Clear()

  oAsmDoc.SelectSet.Select(oSelectedOcc)

 

  ' and execute the built-in command

  m_inventorApplication.CommandManager. _

    ControlDefinitions. _

    Item("SketchProjectCutEdgesCmd").Execute()

End Sub

 

Public Sub CreateCoordSystem(ByRef xVector As Vector, _

                             ByRef yVector As Vector, _

                             ByRef zVector As Vector)

  ' get the transient geometry object

  Dim tg As TransientGeometry = m_inventorApplication. _

    TransientGeometry

  Dim Tolerance As Double = 0.000000000001

 

  'Set a tolerance treshold for the normal vector

  If Math.Abs(zVector.X) < Tolerance Then

    zVector.X = 0.0#

  ElseIf Math.Abs(zVector.Y) < Tolerance Then

    zVector.Y = 0.0#

  ElseIf Math.Abs(zVector.Z) < Tolerance Then

    zVector.Z = 0.0#

  End If

 

  If zVector.X <> 0 Then

    xVector = tg.CreateVector(-zVector.Y / zVector.X, 1, 0)

    yVector = zVector.CrossProduct(xVector)

  ElseIf zVector.Y <> 0 Then

    xVector = tg.CreateVector(0, -zVector.Z / zVector.Y, 1)

    yVector = zVector.CrossProduct(xVector)

  ElseIf zVector.Z <> 0 Then

    xVector = tg.CreateVector(1, 0, 0)

    yVector = zVector.CrossProduct(xVector)

  End If

End Sub