Manufacturing DevBlog

Retrieving Edge.Geometry for linear and circular edges

By Philippe Leefsma

If the Edge is linear, “Edge.CurveType” property returns kLineCurve, the Geometry is a LineSegment, if the Edge is a circle, “Edge.CurveType” returns kCircleCurve, the Geometry is a Circle, if the Edge is a 3D arc, “Edge.CurveType” is still kCircleCurve, but the Geometry is an Arc3d. So when CurveType is kCircleCurve, you may also need to check the object type as follows:

    Sub TestEdgeGeometry(ByVal app As Inventor.Application)

 

        ' assumes an edge is selected

        Dim oEdge As Edge

        oEdge = app.ActiveDocument.SelectSet.Item(1)

 

        If (oEdge.CurveType = CurveTypeEnum.kLineCurve) Then

 

            Dim oLine As Inventor.LineSegment

            oLine = oEdge.Geometry

 

        ElseIf (oEdge.CurveType = CurveTypeEnum.kCircleCurve) Then

 

            If TypeOf oEdge.Geometry Is Inventor.Circle Then

 

                Dim oCir As Inventor.Circle

                oCir = oEdge.Geometry

 

            ElseIf (TypeOf oEdge.Geometry Is Arc3d) Then

 

                Dim oArc As Inventor.Arc3d

                oArc = oEdge.Geometry

 

            End If

 

        End If

 

    End Sub

 

Exporting Flat Pattern as DWG/DXF

By Philippe Leefsma

Q:

How to create a DWG/DXF file flat pattern from an Inventor sheet metal part?

A:

The WriteDataToFile method of the DataIO object supports the option to write the flat pattern out as a DWG file. You can also supply arguments in a method similar to http URL variables (starting with '?', 'key=value', multiple keys and values separated by '&').

The valid arguments are:
TangentLayer = [name]
BendLayer = [name]
OuterProfileLayer = [name]
AcadVersion = {"2005","2004","2002", "2000", "R14", "R13", "R12",} // R12 is only supported for the dxf format type.

For example:

 
"FLAT PATTERN DWG?AcadVersion=2000"
"FLAT PATTERN DWG?AcadVersion=R14"
"FLAT PATTERN DWG?AcadVersion=R13&TangentLayer=myTangLayer"
"FLAT PATTERN DXF?AcadVersion=R14&BendLayer=myBendLayer"

Here is a VB.Net sample:

    Public Sub DwgFlat(ByVal app As Inventor.Application)

 

        Dim oDoc As PartDocument = app.ActiveDocument

        Dim oDataIO As DataIO = oDoc.ComponentDefinition.DataIO

 

        oDataIO.WriteDataToFile(

            "FLAT PATTERN DWG?AcadVersion=2000&BendLayer=myBendLayer",

            "c:\flat.dwg")

 

    End Sub

 

Read Prompted Entry through code

By Barbara Han

Issue

I need to get the property fields which can be seen in "Edit property text" under active Title block. I am able to get other property fields related to drawing through property set, but I don’t how to get the custom property set (Prompted Entry) for Title block.

Solution

The following is a VBA sample code that reads the prompted entry in the title block in the active sheet:

'Before running this code, add reference to Microsoft XML 6.0 in this VBA project

Sub readPromptedEntryInTitleBlock()
    Dim drawing As DrawingDocument
    Set drawing = ThisApplication.ActiveDocument
    Dim tb As TitleBlock
    Set tb = drawing.ActiveSheet.TitleBlock
    Dim textB As TextBox
    For Each textB In tb.Definition.Sketch.TextBoxes
        Dim xml As DOMDocument
        Set xml = New DOMDocument
        Call xml.loadXML(textB.FormattedText)
       
        ' Look for prompted entry
        Dim node As IXMLDOMNode
        Set node = xml.selectSingleNode("Prompt")
        If Not node Is Nothing Then
            Debug.Print node.Text + ":" + tb.GetResultText(textB)
        End If
       
        Set xml = Nothing
    Next
End Sub
 
Actually there is no need to look for the properties from property set, because it’s straight forward to get all texts in the title block through calling TitleBlock.GetResultText() function.

There are some discussion threads talking about the similar issue, for example:
http://forums.autodesk.com/t5/Autodesk-Inventor-Customization/Reading-quot-Prompted-Entry-quot-Title-Block-info-with-VBA/td-p/758297

How to use the AddBaseView method with the Camera parameter ?

By Philippe Leefsma

Q:

I want to create a base drawing view with my own camera parameter. How to get the camera object and set its parameters to use with the "AddBaseView" method?

A:

The following VB.Net code sample illustrates the use of the Camera parameter with the "AddBaseView" method.

Note: The related Part or Assembly document has to be opened in Visible mode in order to retrieve the "Application.ActiveView.Camera" object.

The "ViewOrientation" parameter has to be "kArbitraryViewOrientation" in order to use a custom camera object.

    Sub CreateBaseViewWithCamera(ByVal app As Inventor.Application)

 

        'Open the part to insert in the drawing (Visible mode is required).

 

        Dim oPartDoc As PartDocument =

            app.Documents.Open("C:\Temp\Part1.ipt", True)

 

        'Get Camera object

        Dim oCamera As Camera = app.ActiveView.Camera

 

        'Set your Camera parameters

        oCamera.Eye = app.TransientGeometry.CreatePoint(0, 10, 10)

        oCamera.Target = app.TransientGeometry.CreatePoint(0, 0, 0)

        oCamera.UpVector = app.TransientGeometry.CreateUnitVector(0, 1, 0)

 

        'Open the Drawing doc

        Dim oDrawingDoc As DrawingDocument

        oDrawingDoc = app.Documents.Open(

            "C:\Temp\Drawing1.idw", True)

 

        Dim oSheet As Sheet

        oSheet = oDrawingDoc.Sheets.Item(1)

 

        'Position base view in middle of the sheet

        Dim oViewPos As Point2d

        oViewPos = app.TransientGeometry.CreatePoint2d(

            oSheet.Width / 2, oSheet.Height / 2)

 

        'Create view with parameters

        Dim oBaseView As DrawingView

        oBaseView = oSheet.DrawingViews.AddBaseView(

            oPartDoc,

            oViewPos,

            1,

            ViewOrientationTypeEnum.kArbitraryViewOrientation,

            DrawingViewStyleEnum.kHiddenLineDrawingViewStyle,

            "BaseView1",

            oCamera)

 

        'Close the part doc

        oPartDoc.Close()

 

    End Sub

 

How to find internal command names

By Philippe Leefsma

Q:

I need to find the internal name of a command so I can run it from a macro. Is there an example showing how to find the internal name?

A:

The CommandManager object allows you to run commands as if they were executed from the user interface. The internal name needed (string) for the execute method is not documented in the help file. Here is a VB.Net example that will print out a list of Inventor commands containing "WorkFeatures" in their name:

Sub FindCommandByInternalName(

    ByVal app As Inventor.Application,

    ByVal CommName As String)

 

        'Gets CommandManager's Control Definitions

        Dim oControlDefs As ControlDefinitions

        oControlDefs = app.CommandManager.ControlDefinitions

 

        'Iterates trough all Control Definitions and prints the InternalName and

        'DescriptionText of commands that match a part of the input string

 

        Dim oControlDef As ControlDefinition

        For Each oControlDef In oControlDefs

            If InStr(oControlDef.InternalName, CommName) <> 0 Then

 

                System.Console.WriteLine(

                    "[Internal Name]" & oControlDef.InternalName &

                    " [Description]" & oControlDef.DescriptionText)

 

            End If

        Next

    End Sub

 

    Sub TestCommandName()

 

        FindCommandByInternalName(m_inventorApp, "AppAllWorkfeaturesCmd")

        'This will be printed out in the output window:

        '[Internal Name]AppAllWorkfeaturesCmd

        '[Description]Display all work features (origin and user)

 

    End Sub

 

    Sub TestCommand()

        m_inventorApp.CommandManager.ControlDefinitions.Item

            ("AppAllWorkfeaturesCmd").Execute()

    End Sub

 

How to determine that a user has drawn an object ?

By Philippe Leefsma

Q:

Is there an event or series of events that I can use to determine that the user has drawn an object  such as a line? And find the exact parameters of the object, start point, end point, length, etc.

A:

You can implement the requirement using SketchEvents and DocumentEvents. Use DocumentEvents.OnChange to know why the event fired  such as Create Line, then use SketchEvents. OnSketchChange to know the sketch object.  DocumentEvents.OnChange will be fired before SketchEvents. OnSketchChange is fired.

Here is the VB.Net code:

    Private _ctx As NameValueMap

    Private _docEvents As DocumentEvents

    Private _sketchEvents As SketchEvents

 

    Sub ListenEvents(ByVal app As Inventor.Application)

 

        If (Not app.ActiveDocument Is Nothing) Then

 

            _docEvents = app.ActiveDocument.DocumentEvents

            _sketchEvents = app.SketchEvents

 

            AddHandler _docEvents.OnChange, AddressOf OnDocChange

            AddHandler _sketchEvents.OnSketchChange, AddressOf OnSketchChange

 

        End If

 

    End Sub

 

    Sub OnDocChange(ByVal ReasonsForChange As CommandTypesEnum,

        ByVal BeforeOrAfter As EventTimingEnum,

        ByVal Context As NameValueMap,

        ByRef HandlingCode As HandlingCodeEnum)

 

        If (BeforeOrAfter = EventTimingEnum.kBefore) Then

            _ctx = Context

        End If

 

    End Sub

 

    Sub OnSketchChange(ByVal DocumentObject As Document,

               ByVal Sketch As Sketch,

               ByVal BeforeOrAfter As EventTimingEnum,

               ByVal Context As NameValueMap,

               ByRef HandlingCode As HandlingCodeEnum)

 

        If (BeforeOrAfter = EventTimingEnum.kAfter) Then

            If Sketch.Type = ObjectTypeEnum.kPlanarSketchObject Then

                If _ctx.Item(1) = "Create Line" Then

 

                    Debug.Print("a line is created")

 

                    ' The newest line should be the last item of the

                    ' sketchlines, so use Sketch.SketchLines.count

                    Dim oLine As SketchLine =

                        Sketch.SketchLines.Item(Sketch.SketchLines.Count)

 

 

                    Debug.Print("startPt.x = " & oLine.Geometry.StartPoint.X &

                                " startPt.y = " & oLine.Geometry.StartPoint.Y)

 

                    Debug.Print("EndPt.x = " & oLine.Geometry.EndPoint.X &

                                " startPt.y = " & oLine.Geometry.EndPoint.Y)

 

                End If

            End If

        End If

    End Sub

 

 

Create mate constraint with bias points

By Xiaodong Liang

With the arguments BiasPointOne and BiasPointTwo in AddMateConstraint , the occurrences should be repositioned to make the two bias points coincident. The BiasPoint used by method AddMateConstraint should be from model space. So you need to use the native object of the point to add this constraint. The code below assumes that two faces and two vetex of different occurrences in an assembly context are selected.

Sub constraintWithBiasPoints()

      ' assume we have had the inventor application

    Dim oDoc As Document

    oDoc = _InvApplication.ActiveDocument

 

    Dim oDef As AssemblyComponentDefinition

    oDef = oDoc.ComponentDefinition

 

    Dim oFaceProxy1 As FaceProxy

    Dim oFaceProxy2 As FaceProxy

 

    Dim oPointProxy1 As VertexProxy

    Dim oPointProxy2 As VertexProxy

 

    oFaceProxy1 = oDoc.SelectSet(1)

    oFaceProxy2 = oDoc.SelectSet(2)

    oPointProxy1 = oDoc.SelectSet(3)

    oPointProxy2 = oDoc.SelectSet(4)

 

    oDef.Constraints.AddMateConstraint(oFaceProxy1, _

                                        oFaceProxy2, _

                                        0, _

                 InferredTypeEnum.kNoInference, _

                 InferredTypeEnum.kNoInference, _

                 oPointProxy1.NativeObject.Point, _

                 oPointProxy2.NativeObject.Point) 

End Sub

 

Access the API of the specific version if multi releases on the machine

By Xiaodong Liang

Issue
COM API CocreateInstance is called to get inventor application. If two different Inventor versions( say 2012, 2013) are installed on the same machine. How can we the access the API of the specific version?

Solution
You need to use following workaround.

- Make sure that there is no Inventor.exe running. This can be done using Process.GetProcessesByName

- Start corresponding inventor.exe using Process class

- Use GetActiveObject to get Inventor.Application from process you started. You can use Inventor.SoftwareVersion to find out which version is currently running.

private void test()

{

    bool noInvProcess = true;

    foreach (Process p in

           Process.GetProcessesByName("Inventor"))

    {

        try

        {

            // kill the process

            p.Kill();

            // possibly with a timeout

            p.WaitForExit();         

 

        }

        catch (Exception ex)

        {

            // error

            noInvProcess = false ;

            break;

        }        

    }

 

    if (noInvProcess)

    {

        // assume we want to start inventor 2013

        Process.Start(@"C:\Program Files\Autodesk\Inventor 2013\Bin\Inventor.exe");

 

        // wait a moment

        System.Threading.Thread.Sleep(1000);

 

        // get the active inventor application

        string progId = "Inventor.Application";

        Inventor.Application m_inventorApp =

            (Inventor.Application)Marshal.

             GetActiveObject(progId);

 

        SoftwareVersion oInvVer = m_inventorApp.SoftwareVersion;

        MessageBox.Show("current running inventor is : " + oInvVer.Major);

    }

}

find corresponding source face on defived part

By Xiaodong Liang

Issue
I have part and derived part based on it. I need to
  1. get the base face from derived face
  2. get derived face from base face

Solution

1. You can use Face.ReferencedEntity to get the face of base part. Note: Face.ReferencedEntity could be one face or faces. 

2. You can
    1) use oBaseDoc.ReferencingDocuments to find which file is referenced from the source file.
    2) Iterate each derived components in the derived document and find which component is referenced from the source file
    3) Iterate each face in the derived component and find which Face.ReferencedEntity is the source face

' get the base face from derived face

Sub getBaseFace()

 

     ' assume we have got Inventor application   

    Dim oDerivedDoc As PartDocument

    oDerivedDoc = _InvApplication.ActiveDocument

 

    ' assume a face in derived document is selected

    Dim oDerivedFace As Face

    oDerivedFace = oDerivedDoc.SelectSet(1)

 

    Dim oDerivedDocDef As PartComponentDefinition

    oDerivedDocDef = oDerivedDoc.ComponentDefinition

 

    ' get the DerivedPartComponent

    Dim oDerivedC As DerivedPartComponent

    oDerivedC = _

        oDerivedDocDef.ReferenceComponents. _

        DerivedPartComponents(1)

 

    ' get the base document

    Dim oBaseDoc As PartDocument

    oBaseDoc = _

        _InvApplication.Documents.Open( _

        oDerivedC.ReferencedDocumentDescriptor.FullDocumentName, _

        False)

 

    ' get ComponentDefinition of the base part

    Dim oBaseDef As PartComponentDefinition

    oBaseDef = oBaseDoc.ComponentDefinition

 

    Dim oBaseFace As Face

    Dim tempFace As Face

 

    ' check which base face is corresponding to the

    ' derived face

    For Each oBaseFace In _

        oBaseDef.SurfaceBodies(1).Faces

        Try

            tempFace = oDerivedFace.ReferencedEntity

            'referenced entity is one face

            If tempFace Is oBaseFace Then

                Debug.Print("found the source face!")

            End If

        Catch ex As Exception

            ' referenced entity is faces collection

            For Each tempFace In oDerivedFace.ReferencedEntity

                If tempFace Is oBaseFace Then

                    Debug.Print("found the source (base) face!")

                End If

            Next

        End Try

    Next

 

    oBaseDoc.Close()

 

End Sub

 

 '  get derived face from base face.

Sub getDerivedFace()

 

     ' assume we have got Inventor application   

 

    ' assume the base document is opened

    Dim oBaseDoc As PartDocument

    oBaseDoc = _InvApplication.ActiveDocument

 

    ' assume a face in the base document is selected

    Dim oBaseFace As Face

    oBaseFace = oBaseDoc.SelectSet(1)

 

    ' iterate each Referencing document(derived document)

 

    Dim oReferencingDoc As PartDocument

    For Each oReferencingDoc In  _

        oBaseDoc.ReferencingDocuments

 

        ' get ComponentDefinition of the derived document

        Dim oReferencingDocDef As PartComponentDefinition

        oReferencingDocDef = oReferencingdDoc.ComponentDefinition

 

        Dim oDerivedC As DerivedPartComponent

        For Each oDerivedC In _

            oReferencingDocDef.ReferenceComponents. _

            DerivedPartComponents

 

            ' find what derived component is from the base doc

            If oDerivedC.ReferencedDocumentDescriptor. _

                FullDocumentName = oBaseDoc.FullDocumentName Then

 

                Dim oDerivedFace As Face

                Dim tempFace As Face

 

                For Each oDerivedFace In oDerivedC.PrimaryBody.Faces

                        Try

                        tempFace = oDerivedFace.ReferencedEntity

                        'referenced entity is one face

                        If tempFace Is oBaseFace Then

                            Debug.Print( _

                                "found the derived face!")

                        End If

                    Catch ex As Exception

                        ' referenced entity is faces collection

                        For Each tempFace In  _

                            oDerivedFace.ReferencedEntity

                            If tempFace Is oBaseFace Then

                                Debug.Print( _

                                    "found the derived face!")

                            End If

                        Next

                    End Try

                Next

            End If

 

        Next

    Next

End Sub

Load iges or Parasolid files into the active Inventor document

By Xiaodong Liang

Issue
I want to load iges or parasolid files into the active document of Inventor via the api. I want this to work in the same way as the [Import] command in Inventor. The code below works but does not load the iges file into the active document, it creates its own file.

Solution
The argument “TargetObject” of TranslatorAddIn.Open has to use the new document. There's an easy way to do this with Inventor 2011. Use NonParametricBaseFeatures.Add to create a base feature in the desired part file. But it is as designed that NonParametricBaseFeatures.Add should create a solid if there are no other solids in the part and a surface if there is at least one solid in the part. So if batching importing, the next file will be imported as surface. To have all as solid, you could use CreateDefinition and AddByDefinition methods of the NonParametricBaseFeatures object which were added in Inventor 2011 and support additional capabilities that the Add method doesn’t. The code below imports ttwo Parasolid files to the current part.

Sub testImport()

 

' import file 1

ImportXB ("C:\Temp\1.X_B")

' import file 2

ImportXB ("C:\Temp\2.X_B" )

 

End Sub

 

' import function

Sub ImportXB(fileName As String)

 

     ' assume we have got Inventor application   

 

    ' get active document

    Dim oActiveDoc As PartDocument = _

         _InvApplication.ActiveDocument

 

    ' get  ComponentDefinition

    Dim oActiveDocDef As PartComponentDefinition = _

        oActiveDoc.ComponentDefinition

 

    ' get the  TranslatorAddIn

    Dim oAddin As TranslatorAddIn = _

        _InvApplication.ApplicationAddIns. _

        ItemById("{A8F8F8E5-BBAB-4F74-8B1B-AC011251F8AC}")

 

    ' prepare the arguments for  TranslatorAddIn  

    Dim oContext As TranslationContext = _

          _InvApplication.TransientObjects. _

          CreateTranslationContext

 

    oContext.Type = _

        IOMechanismEnum.kFileBrowseIOMechanism 

 

    Dim oOptions As NameValueMap = _

        _InvApplication.TransientObjects. _

        CreateNameValueMap

 

    Dim oDataMedium As DataMedium = _ 

        _InvApplication.TransientObjects.CreateDataMedium

 

    ' set the option ImportSolid = true

     oOptions.Add("ImportSolid", True)

 

     oDataMedium.fileName = fileName

 

    ' import the file to one new part document

    Dim oNewDoc As PartDocument

    oAddin.Open(oDataMedium, oContext, oOptions, oNewDoc)

 

    oNewDoc.Views.Add

 

    ' get PartComponentDefinition of the new part document        

    Dim oNewDocDef As PartComponentDefinition = _

        oNewDoc.ComponentDefinition

 

    ' create one Definition of NonParametricBaseFeature

    Dim oNPFD As NonParametricBaseFeatureDefinition = _

        oActiveDocDef.Features.NonParametricBaseFeatures. _

        CreateDefinition

 

    Dim oObjColl As ObjectCollection = _

        _InvApplication.TransientObjects.CreateObjectCollection()

 

    ''check the solids

    Dim oSB As SurfaceBody

    For Each oSB In oNewDocDef.SurfaceBodies

        oObjColl.Add (oSB)

    Next

 

    oNPFD.BRepEntities = oObjColl

    oNPFD.OutputType =BaseFeatureOutputTypeEnum.kSolidOutputType

 

    ' add the bodies of the new part document to the

    ' active document

    oActiveDocDef.Features.NonParametricBaseFeatures. _

        AddByDefinition( oNPFD  )

 

    'close the temp doc without saving

    ' because we do not need it any more

    oNewDoc.Close( True)

 

End Sub