Manufacturing DevBlog

Import specific layers of DWG to inventor part sketch

By Xiaodong Liang

The option SelectedLayout of the Translator Addin of DWG can specify the layers to import to the sketch.

oOptions.Add "SelectedLayers", "Layer1"

you can also specify several layers, e.g.

oOptions.Add "SelectedLayers", "Layer1,Layer2" 

Sub ImportDWGIntoSketch()
    'DWG translator
    Dim oDwg As TranslatorAddIn
    Set oDwg = ThisApplication.ApplicationAddIns.ItemById("{C24E3AC2-122E-11D5-8E91-0010B541CD80}")
    Dim oData As DataMedium
    Dim oContext As TranslationContext
    Dim oOptions As NameValueMap
    Set oData = ThisApplication.TransientObjects.CreateDataMedium
    Set oContext = ThisApplication.TransientObjects.CreateTranslationContext
    Set oOptions = ThisApplication.TransientObjects.CreateNameValueMap
    ' Specify a DWG file to import it into sketch, please change the path name as needed
    oData.FileName = "C:\Temp\mytest.dwg"
    Dim oDoc As PartDocument
    Set oDoc = ThisApplication.Documents.Add(kPartDocumentObject)
    'add a new sketch
    Dim oSk As PlanarSketch
    Set oSk = oDoc.ComponentDefinition.Sketches.Add(oDoc.ComponentDefinition.WorkPlanes(3))
    oSk.Edit
    oContext.Type = kFileBrowseIOMechanism
    oContext.OpenIntoExisting = oSk

    ' Specify the layers to import
  oOptions.Add "SelectedLayers", "Layer1" 
  ‘oOptions.Add "SelectedLayers", "0,Layer2" 
    oOptions.Add "InvertLayersSelection", False ' Set if import the selected layers in above setting
    ' Set the ConstrainEndPoints
    oOptions.Add "ConstrainEndPoints", True
    ' Specify the units of DWG file
    oOptions.Add "FileUnits", "Millimeters"
    Call oDwg.Open(oData, oContext, oOptions, oDoc)
End Sub

2014 Product Line Unveiled

By Adam Nagy

You can find many websites talking about the unveiling of the 2014 Autodesk products. Here is the video of the announcement: http://www.youtube.com/watch?v=w-kxV8C4xro

There are also various sites discussing the new features of the coming product releases. But if you are interested in the API side of things, then you can have a look at Brian's first post on the Inventor 2014 API Enhancements. 

 

Hook up a chain using iMate's

By Adam Nagy

When constraining parts together in an assembly, if you organized things well then with a bit of programming you can automate things nicely.

You could use iMate's to specify how the parts should be contrained to each other - this would be just a one off thing so could be done in the user interface as well. Then you could programmatically insert multiple instances of them (same number of each) and use the iMate's to join them.

In this case we have two parts of a chain assembly. Each have the same iMate's: iMate:1 and iInsert:1 on one end of the part, and iMate:2 and iInsert:2 on the other end of the part. We could pair them like this:

This code assumes that there are the same number of occurrences of each part in the assembly already and none of the iMate's have been used:

Function GetiMate(name As String, occ As ComponentOccurrence) _
As iMateDefinition
    Dim imate As iMateDefinition
    For Each imate In occ.iMateDefinitions
        If imate.name = name Then
            Set GetiMate = imate
            Exit Function
        End If
    Next
End Function

' This hooks "chain1" parts to "chain2" parts
' In this assembly we only have these two parts
' so checking if the part documents are not the
' same is enough
Sub HookTheChain()
    Dim doc As AssemblyDocument
    Set doc = ThisApplication.ActiveDocument
    
    Dim cd As AssemblyComponentDefinition
    Set cd = doc.ComponentDefinition
    
    ' Here we only have two referenced files
    Dim desc1 As DocumentDescriptor
    Set desc1 = doc.ReferencedDocumentDescriptors(1)
    Dim occs1 As ComponentOccurrencesEnumerator
    Set occs1 = cd.Occurrences.AllReferencedOccurrences(desc1)
    
    Dim desc2 As DocumentDescriptor
    Set desc2 = doc.ReferencedDocumentDescriptors(2)
    Dim occs2 As ComponentOccurrencesEnumerator
    Set occs2 = cd.Occurrences.AllReferencedOccurrences(desc2)
    
    Dim i As Integer
    For i = 1 To occs1.Count
        ' Set occ1 iMate:1/iInsert:1 to
        ' occ2 iMate:1/iInsert:1
        Dim imate1 As iMateDefinition
        Set imate1 = GetiMate("iMate:1", occs1(i))
        Dim imate2 As iMateDefinition
        Set imate2 = GetiMate("iMate:1", occs2(i))
        
        Call cd.iMateResults.AddByTwoiMates(imate1, imate2)
        
        Set imate1 = GetiMate("iInsert:1", occs1(i))
        Set imate2 = GetiMate("iInsert:1", occs2(i))
        
        Call cd.iMateResults.AddByTwoiMates(imate1, imate2)
        
        ' Set occ1 iMate:2/iInsert:2 to
        ' another occ2 iMate:2/iInsert:2
        Dim ip1 As Integer
        ip1 = i Mod occs2.Count + 1
        
        Set imate1 = GetiMate("iMate:2", occs1(i))
        Set imate2 = GetiMate("iMate:2", occs2(ip1))
        
        Call cd.iMateResults.AddByTwoiMates(imate1, imate2)
        
        Set imate1 = GetiMate("iInsert:2", occs1(i))
        Set imate2 = GetiMate("iInsert:2", occs2(ip1))
        
        Call cd.iMateResults.AddByTwoiMates(imate1, imate2)
    Next
End Sub

Once you run the code the parts might end up on top of each other, but when you drag them using the mouse then you'll see that they can be moved and are hooked up as intended:

Parts and assembly files are attached in the zip - Download Chain. You can just open up the assembly and run the above code.  

Allow custom values setting of a parameter

By Adam Nagy

In the user interface this is where you can set the Allow custom values option for a parameter:

In case of the API, you'll find it in a custom Attribute:

Here is a VBA sample that toggles this value for the first user parameter if possible:

Sub Toggle_AllowCustomValue()
    Dim doc As PartDocument
    Set doc = ThisApplication.ActiveDocument
    
    Dim pcd As PartComponentDefinition
    Set pcd = doc.ComponentDefinition
    
    Dim p As UserParameter
    Set p = pcd.Parameters.UserParameters(1)
    
    On Error Resume Next
    
    Dim att As Inventor.Attribute
    Set att = p.AttributeSets _
        ("com.autodesk.inventor.ParameterAttributes") _
        ("AllowCustomValue")
    
    If Not att Is Nothing Then
        att.Value = Not att.Value
    End If
    
    On Error GoTo 0
End Sub

Show up-to-date loop length

By Adam Nagy

Through the user interface you can query the length of an entity loop using the Measure Loop tool (Tools >> Measure >> Loop)

If you want to keep showing the length of a specific loop, e.g. in the sketch environment, while editing the geometry, you can do that from your AddIn or VBA. In this case I created a form class in VBA called LengthForm, with a Label (named LengthValue) and a Button (named MarkEntity) on it and used the following code.
Note that this part of the code is for the form that you've just created. Right-click on the LengthForm in the Project window's tree and select View Code - that's where this code should be pasted.

Private WithEvents docEvents As DocumentEvents
Private selEnt As Object

Private Sub docEvents_OnChange( _
ByVal ReasonsForChange As CommandTypesEnum, _
ByVal BeforeOrAfter As EventTimingEnum, _
ByVal Context As NameValueMap, _
HandlingCode As HandlingCodeEnum)
    If BeforeOrAfter <> kAfter Then Exit Sub
    
    LengthValue.Caption = GetLength(selEnt)
End Sub

Private Sub MarkEntity_Click()
    Dim ss As SelectSet
    Set ss = ThisApplication.ActiveDocument.SelectSet
    
    If ss.Count = 0 Then
        Set docEvents = Nothing
        
        LengthValue.Caption = ""
    Else
        Set docEvents = _
            ThisApplication.ActiveDocument.DocumentEvents
            
        Set selEnt = ss(1)
        LengthValue.Caption = GetLength(selEnt)
    End If
End Sub

Function GetLength(ent As Object) As String
    Dim l As Double
    ' Try this
    'l = ThisApplication.MeasureTools.GetLoopLength(ent)
    ' Or this
    l = GetFirstLoopLength(ent)
    
    ' Internal length unit is cm
    GetLength = str(l) + " cm"
End Function

' This is using own logic
Function GetFirstLoopLength(ByVal ent As SketchEntity) As Double
    If ent Is Nothing Then Exit Function
    
    Dim ents As ObjectCollection
    Set ents = ThisApplication.TransientObjects.CreateObjectCollection
    
    Call ents.Add(ent)
    
    Dim success As Boolean
    success = GetFirstLoopRec(ent, ent.EndSketchPoint, ents)
    
    If success Then
        Dim l As Double
        For Each ent In ents
            l = l + ent.Length
        Next
        
        GetFirstLoopLength = l
    End If
End Function

' Return True means we're done
Function GetFirstLoopRec(prev As SketchEntity, sp As SketchPoint, _
ents As ObjectCollection) As Boolean
     Dim first As Object
     Set first = ents(1)
     
     Dim ent As SketchLine
     For Each ent In sp.OwnedBy
        ' If it's not the same as the previuos
        ' entity
        If Not ent Is prev Then
            ' If it's the same as the first entity
            ' then we made a loop
            If ent Is first Then
                GetFirstLoopRec = True
                Exit Function
            End If
            
            Call ents.Add(ent)
            ' Get the sketch point on the other
            ' side of this entity
            If ent.StartSketchPoint Is sp Then
                If GetFirstLoopRec( _
                ent, ent.EndSketchPoint, ents) Then
                    GetFirstLoopRec = True
                    Exit Function
                End If
            Else
                If GetFirstLoopRec( _
                ent, ent.StartSketchPoint, ents) Then
                    GetFirstLoopRec = True
                    Exit Function
                End If
            End If
        End If
     Next
     
     GetFirstLoopRec = False
End Function

Now I can show it modelessly, so that it is always visible. 

Dim lf As LengthForm

Sub ShowLengthForm()
    Set lf = New LengthForm
    lf.Show vbModeless
End Sub

When testing the code, first select a sketch entity that is part of a loop, and then click Mark Entity.

Note: the ThisApplication.MeasureTools.GetLoopLength(ent) function did not always find the loop. My own function seems to work fine, but I did not thoroughly test it.

Evaluator of EdgeUse vs Edge

By Adam Nagy

EdgeUse is an object that provides information in context of one of the Face's the Edge belongs to. The Curve2dEvaluator you get from this object's Evaluator property also provides information in context of the Face, which also means that the returned coordinates are in the parametric space of the Face (u, v). 
If you want to get the model coordinates of a point then you can use the Face's Evaluator to convert the u,v coordinates to model coordinates (x, y, z) 

Edge on the other hand provides information in context of the model space, and the Curve2dEvaluator you get from its Evaluator property returns model space coordinates.

The following is a sample with made up coordinates - in a real case the 0 u,v coordinates might not be at the start of a Face or Edge - you need to retrieve the minimum/maximum values using the appropriate functions.

 

Here is a VBA code that shows the relation between the EdgeUse Evaluator's u coordintate, the Face's u, v coordinates and the model space coordinates - select a face before running the code:

Sub PlaceParametricPoints()
    Dim oDoc As PartDocument
    Set oDoc = ThisApplication.ActiveDocument

    Dim oFace As Face
    Set oFace = oDoc.SelectSet(1)
    
    Dim oCompDef As PartComponentDefinition
    Set oCompDef = oDoc.ComponentDefinition
    
    Dim oWPs As WorkPoints
    Set oWPs = oCompDef.WorkPoints
    
    Dim oEdgeLoop As EdgeLoop
    For Each oEdgeLoop In oFace.EdgeLoops
        Dim oEdgeUse As EdgeUse
        For Each oEdgeUse In oEdgeLoop.EdgeUses
            Dim oEval As Curve2dEvaluator
            Set oEval = oEdgeUse.Evaluator
            
            ' Get min and max point in
            ' parametric space of curve
            Dim oMinU As Double
            Dim oMaxU As Double
            Call oEval.GetParamExtents(oMinU, oMaxU)
            
            ' Get the same points in the parametric
            ' space of the face
            Dim oParams(1) As Double
            Dim oFaceUV() As Double
            oParams(0) = oMinU
            oParams(1) = oMaxU
            Call oEval.GetPointAtParam(oParams, oFaceUV)
            
            ' Get the same points in the model coordinate
            ' system
            Dim oModel() As Double
            Call oFace.Evaluator.GetPointAtParam(oFaceUV, oModel)
            
            Dim oTG As TransientGeometry
            Set oTG = ThisApplication.TransientGeometry
            

            Call oWPs.AddFixed(oTG.CreatePoint( _
                oModel(0), oModel(1), oModel(2)))
            
            Debug.Print _
                "> Min Point >>>>>>>>>>>>>>>>>>>>>>>>>>>>>>" + vbCrLf + _
                " Edge  u = " + str(oMinU) + vbCrLf + _
                " Face  u = " + str(oFaceUV(0)) + _
                ", v = " + str(oFaceUV(1)) + vbCrLf + _
                " Model x = " + str(oModel(0)) + _
                ", y = " + str(oModel(1)) + _
                ", z = " + str(oModel(2)) + vbCrLf + _
                "> Max Point >>>>>>>>>>>>>>>>>>>>>>>>>>>>>>" + vbCrLf + _
                " Edge  u  = " + str(oMaxU) + vbCrLf + _
                " Face  u  = " + str(oFaceUV(2)) + _
                ", v = " + str(oFaceUV(3)) + vbCrLf + _
                " Model x = " + str(oModel(3)) + _
                ", y = " + str(oModel(4)) + _
                ", z = " + str(oModel(5))
        Next
    Next
End Sub

Have a look at the following document for more information: modthemachine.typepad.com/files/mathgeometry.pdf 

Replace Dimension Style

By Adam Nagy

When you right-click on a Dimension style in the Style and Standard Editor dialog, then you can select Replace Style. This will go through all the local Object Defaults and check if the given Dimension style is used by any of its dimension related settings (Angle Dimension, Baseline Dimension Set, Bend Note, etc) which have the dimension icon next to them. The ones that are using the selected Dimension style will be adjusted to use the other Dimension style you provided in the Replace Style dialog.

You can do the same programmatically. You can go through all the local ObjectDefaultsStyle objects and check their Dimension related properties, either by hard-coding them in your program or doing it using COM Type Information. This sample shows both.

using System;

using System.Reflection;

using System.Runtime.InteropServices;

using CT = System.Runtime.InteropServices.ComTypes;

 

using Inventor;

 

namespace TestConsole

{

  class Program

  {

    #region Dynamic

    [ComImport()]

    [Guid("00020400-0000-0000-C000-000000000046")]

    [InterfaceType(ComInterfaceType.InterfaceIsIUnknown)]

    public interface IDispatch

    {

      [PreserveSig]

      int GetTypeInfoCount(out int Count);

 

      [PreserveSig]

      int GetTypeInfo

          (

              [MarshalAs(UnmanagedType.U4)] int iTInfo,

              [MarshalAs(UnmanagedType.U4)] int lcid,

              out CT.ITypeInfo typeInfo

          );

 

      [PreserveSig]

      int GetIDsOfNames

          (

              ref Guid riid,

              [MarshalAs(UnmanagedType.LPArray,

                ArraySubType = UnmanagedType.LPWStr)]

            string[] rgsNames,

              int cNames,

              int lcid,

              [MarshalAs(UnmanagedType.LPArray)] int[] rgDispId

          );

 

      [PreserveSig]

      int Invoke

          (

              int dispIdMember,

              ref Guid riid,

              uint lcid,

              ushort wFlags,

              ref CT.DISPPARAMS pDispParams,

              out object pVarResult,

              ref CT.EXCEPINFO pExcepInfo,

              IntPtr[] pArgErr

          );

    }

 

    class COMIDispatch

    {

      public enum MethodType

      {

        Method = 0,

        Property_Getter = 1,

        Property_Putter = 2,

        Property_PutRef = 3

      }

 

      public struct MethodInformation

      {

        public string m_strName;

        public string m_strDocumentation;

        public MethodType m_method_type;

      }

 

      // This static function returns an array containing

      // information of all public methods of a COM object.

      // Note that the COM object must implement the IDispatch

      // interface in order to be usable in this function.

      public static MethodInformation[]

        GetMethodInformation(object com_obj)

      {

        IDispatch pDispatch = null;

 

        try

        {

          // Obtain the COM IDispatch interface from the input

          // com_obj object.

          // Low-level-wise this causes a QueryInterface() to be

          // performed on com_obj to obtain the IDispatch interface

          // from it.

          pDispatch = (IDispatch)com_obj;

        }

        catch (System.InvalidCastException)

        {

          // This means that the input com_obj

          // does not support the IDispatch

          // interface.

          return null;

        }

 

        // Obtain the ITypeInfo interface from the object via its

        // IDispatch.GetTypeInfo() method.

        CT.ITypeInfo pTypeInfo = null;

        // Call the IDispatch.GetTypeInfo() to obtain an ITypeInfo

        // interface pointer from the com_obj.

        // Note that the first parameter must be 0 in order to

        // obtain the Type Info of the current object.

        pDispatch.GetTypeInfo

        (

            0,

            0,

            out pTypeInfo

        );

 

        // If for some reason we are not able to obtain the

        // ITypeInfo interface from the IDispatch interface

        // of the COM object, we return immediately.

        if (pTypeInfo == null)

        {

          return null;

        }

 

        // Get the TYPEATTR (type attributes) of the object

        // via its ITypeInfo interface.

        IntPtr pTypeAttr = IntPtr.Zero;

        CT.TYPEATTR typeattr;

        // The TYPEATTR is returned via an IntPtr.

        pTypeInfo.GetTypeAttr(out pTypeAttr);

        // We must convert the IntPtr into the TYPEATTR structure

        // defined in the System.Runtime.InteropServices.ComTypes

        // namespace.

        typeattr = (CT.TYPEATTR)Marshal.PtrToStructure

            (

              pTypeAttr,

              typeof(CT.TYPEATTR)

            );

        // Release the resources related to the obtaining of the

        // COM TYPEATTR structure from an ITypeInfo interface.

        // From now onwards, we will only work with the

        // System.Runtime.InteropServices.ComTypes.TYPEATTR

        // structure.

        pTypeInfo.ReleaseTypeAttr(pTypeAttr);

        pTypeAttr = IntPtr.Zero;

 

        // The TYPEATTR.guid member indicates the default interface

        // implemented by the COM object.

        Guid defaultInterfaceGuid = typeattr.guid;

 

        MethodInformation[] method_information_array =

          new MethodInformation[typeattr.cFuncs];

        // The TYPEATTR.cFuncs member indicates the total number of

        // methods that the current COM object implements.

        for (int i = 0; i < (typeattr.cFuncs); i++)

        {

          // We loop through the number of methods.

          CT.FUNCDESC funcdesc;

          IntPtr pFuncDesc = IntPtr.Zero;

          string strName;

          string strDocumentation;

          int iHelpContext;

          string strHelpFile;

 

          // During each loop, we use the ITypeInfo.GetFuncDesc()

          // method to obtain a FUNCDESC structure which describes

          // the current method indexed by "i".

          pTypeInfo.GetFuncDesc(i, out pFuncDesc);

          // The FUNCDESC structure is returned as an IntPtr.

          // We need to convert it into a FUNCDESC structure

          // defined in the System.Runtime.InteropServices.ComTypes

          // namespace.

          funcdesc = (CT.FUNCDESC)Marshal.PtrToStructure

              (

                pFuncDesc,

                typeof(CT.FUNCDESC)

              );

          // The FUNCDESC.memid contains the member id of the current

          // function in the Type Info of the object.

          // Use the ITypeInfo.GetDocumentation() with reference to

          // memid to obtain information for this function.

          pTypeInfo.GetDocumentation

              (

                funcdesc.memid,

                out strName,

                out strDocumentation,

                out iHelpContext,

                out strHelpFile

              );

          // Fill up the appropriate method_information_array element

          // with field information.

          method_information_array[i].m_strName = strName;

          System.Diagnostics.Debug.WriteLine(strName);

          method_information_array[i].m_strDocumentation =

            strDocumentation;

 

          if (funcdesc.invkind == CT.INVOKEKIND.INVOKE_FUNC)

          {

            method_information_array[i].m_method_type =

              MethodType.Method;

          }

          else if (funcdesc.invkind ==

            CT.INVOKEKIND.INVOKE_PROPERTYGET)

          {

            method_information_array[i].m_method_type =

              MethodType.Property_Getter;

          }

          else if (funcdesc.invkind ==

            CT.INVOKEKIND.INVOKE_PROPERTYPUT)

          {

            method_information_array[i].m_method_type =

              MethodType.Property_Putter;

          }

          else if (funcdesc.invkind ==

            CT.INVOKEKIND.INVOKE_PROPERTYPUTREF)

          {

            method_information_array[i].m_method_type =

              MethodType.Property_PutRef;

          }

 

          // The ITypeInfo.ReleaseFuncDesc() must be called

          // to release the (unmanaged) memory of the FUNCDESC

          // returned in pFuncDesc (an IntPtr).

          pTypeInfo.ReleaseFuncDesc(pFuncDesc);

          pFuncDesc = IntPtr.Zero;

        }

 

        return method_information_array;

      }

    }

 

    static void ReplaceDimensionStyle_Dynamic(

      DrawingStylesManager stylesManager,

      DimensionStyle replaceStyle,

      DimensionStyle withStyle,

      bool purge)

    {

      foreach (ObjectDefaultsStyle defaultStyle

        in stylesManager.ObjectDefaultsStyles)

      {

        if (defaultStyle.StyleLocation ==

          StyleLocationEnum.kLibraryStyleLocation)

          continue;

 

        // Get all the properties of the object

        COMIDispatch.MethodInformation [] methodInfos =

          COMIDispatch.GetMethodInformation(defaultStyle);

 

        foreach (

          COMIDispatch.MethodInformation methodInfo in methodInfos)

        {

          if (methodInfo.m_method_type ==

            COMIDispatch.MethodType.Property_Getter)

          {

            object obj = defaultStyle.GetType().InvokeMember(

                methodInfo.m_strName, BindingFlags.GetProperty, null,

                defaultStyle, null);

 

            if (obj == replaceStyle)

            {

              defaultStyle.GetType().InvokeMember(

                methodInfo.m_strName, BindingFlags.SetProperty, null,

                defaultStyle, new object[] { withStyle });

            }

          }

        }

      }

 

      if (purge && replaceStyle.StyleLocation !=

        StyleLocationEnum.kLibraryStyleLocation)

        replaceStyle.Delete();

    }

    #endregion

 

    #region Hard-Coded

    static void ReplaceDimensionStyle_HardCoded(

      DrawingStylesManager stylesManager,

      DimensionStyle replaceStyle,

      DimensionStyle withStyle,

      bool purge)

    {

      foreach (ObjectDefaultsStyle defaultStyle

        in stylesManager.ObjectDefaultsStyles)

      {

        if (defaultStyle.StyleLocation ==

          StyleLocationEnum.kLibraryStyleLocation)

          continue;

 

        if (defaultStyle.AngularDimensionStyle == replaceStyle)

          defaultStyle.AngularDimensionStyle = withStyle;

 

        if (defaultStyle.BaselineDimensionStyle == replaceStyle)

          defaultStyle.BaselineDimensionStyle = withStyle;

 

        if (defaultStyle.BendNoteStyle == replaceStyle)

          defaultStyle.BendNoteStyle = withStyle;

 

        if (defaultStyle.BendTagStyle == replaceStyle)

          defaultStyle.BendTagStyle = withStyle;

 

        if (defaultStyle.ChainDimensionStyle == replaceStyle)

          defaultStyle.ChainDimensionStyle = withStyle;

 

        if (defaultStyle.ChamferNoteStyle == replaceStyle)

          defaultStyle.ChamferNoteStyle = withStyle;

 

        if (defaultStyle.DiameterDimensionStyle == replaceStyle)

          defaultStyle.DiameterDimensionStyle = withStyle;

 

        if (defaultStyle.HoleNoteStyle == replaceStyle)

          defaultStyle.HoleNoteStyle = withStyle;

 

        if (defaultStyle.HoleTagStyle == replaceStyle)

          defaultStyle.HoleTagStyle = withStyle;

 

        if (defaultStyle.LeaderTextStyle == replaceStyle)

          defaultStyle.LeaderTextStyle = withStyle;

 

        if (defaultStyle.LinearDimensionStyle == replaceStyle)

          defaultStyle.LinearDimensionStyle = withStyle;

 

        if (defaultStyle.OrdinateDimensionStyle == replaceStyle)

          defaultStyle.OrdinateDimensionStyle = withStyle;

 

        if (defaultStyle.OrdinateSetDimensionStyle == replaceStyle)

          defaultStyle.OrdinateSetDimensionStyle = withStyle;

 

        if (defaultStyle.PunchNoteStyle == replaceStyle)

          defaultStyle.PunchNoteStyle = withStyle;

 

        if (defaultStyle.RadialDimensionStyle == replaceStyle)

          defaultStyle.RadialDimensionStyle = withStyle;

 

        if (defaultStyle.ThreadNoteStyle == replaceStyle)

          defaultStyle.ThreadNoteStyle = withStyle;

      }

 

      if (purge && replaceStyle.StyleLocation !=

        StyleLocationEnum.kLibraryStyleLocation)

        replaceStyle.Delete();

    }

    #endregion

 

    static private void test()

    {

      const bool useHardCoded = true;

 

      Application app = (Application)

        System.Runtime.InteropServices.Marshal.

        GetActiveObject("Inventor.Application");

 

      DrawingDocument dwg = (DrawingDocument)app.ActiveDocument;

 

      COMIDispatch.MethodInformation[] methodInfos =

          COMIDispatch.GetMethodInformation(

          dwg.StylesManager.ObjectDefaultsStyles[1]);

 

      DrawingStylesManager stylesManager = dwg.StylesManager;

 

      DimensionStyle style1 = stylesManager.DimensionStyles[1];

      DimensionStyle style2 = stylesManager.DimensionStyles[2];

      if (useHardCoded)

        ReplaceDimensionStyle_HardCoded(

          stylesManager, style1, style2, true);

      else

        ReplaceDimensionStyle_Dynamic(

          stylesManager, style1, style2, true);

    }

 

    static void Main(string[] args)

    {

      test();

    }

  }

}

 

Save extra data in Inventor file – 3

By Xiaodong Liang

Note: the solution in this article uses the the wrapped functions of Inventor API with IStorage and IStream which require to make the document dirty. If you do not need Inventor API, please refer to the other article. 

Inventor files are also a kind of Windows files. Windows API allows you attach data to the file, which is called IStorage & IStream. The other post tells in detail, including the C++ demo code.

How to use private storage and stream in C++

So, I was ready to post the equivalent .NET codes. Actually, I had such discussion on the forum a few months ago:

http://forums.autodesk.com/t5/Autodesk-Inventor-Customization/Store-object-inside-document/td-p/3610956

in which, I have written out some codes. It works well with creating, unfortunately however it failed with reading. I was stuck and the reason was not clear to me.

These days,  my colleague Mona in the engineer team kindly offered a hand on this issue. She finally found the private storage failed to get again is because of it being locked. The IStorage pointer is not released when creating the private storage for the first time. Then for the second time to get it, it’s considered as locked. The way to solve it is to release the pointer before it is called next time, by “Marshal.ReleaseComObject(pStg);” It is the developer’s responsibility to release it. C++ code is lucky since the demo uses smart pointer which can release it for you.

Thanks Mona so much for the solution!  Now, the code works :) And thanks again for these two articles which helped me a lot.

 http://www.pinvoke.net/default.aspx/Enums/STGM.html
http://bytes.com/topic/c-sharp/answers/760093-accessing-com-c-istream-parameter

using System;

using System.Collections.Generic;

using System.ComponentModel;

using System.Data;

using System.Drawing;

using System.Linq;

using System.Text;

using System.Windows.Forms;

using System.Runtime.InteropServices;

using System.Reflection;

using Inventor;

using System.Diagnostics;

using MVOI = Microsoft.VisualStudio.OLE.Interop;

 

        //enum flags for STGM

        [Flags]

        publicenumSTGM : int

        {

            DIRECT = 0x00000000,

            TRANSACTED = 0x00010000,

            SIMPLE = 0x08000000,

            READ = 0x00000000,

            WRITE = 0x00000001,

            READWRITE = 0x00000002,

            SHARE_DENY_NONE = 0x00000040,

            SHARE_DENY_READ = 0x00000030,

            SHARE_DENY_WRITE = 0x00000020,

            SHARE_EXCLUSIVE = 0x00000010,

            PRIORITY = 0x00040000,

            DELETEONRELEASE = 0x04000000,

            NOSCRATCH = 0x00100000,

            CREATE = 0x00001000,

            CONVERT = 0x00020000,

            FAILIFTHERE = 0x00000000,

            NOSNAPSHOT = 0x00200000,

            DIRECT_SWMR = 0x00400000,

        }

 

        // create private storage and stream

        bool  CreatePrivateStorageAndStream(Document pDoc,

            string StorageName,

            string StreamName,

            string data)

        {

            try

            {

                // create/get storage. "true" means if create
               //if it does not exists.

                MVOI.IStorage pStg =

                    (MVOI.IStorage)pDoc.GetPrivateStorage
                                        (StorageName, true);

                if (pStg == null)

                    returnfalse;

 

                // create stream in the storage

                MVOI.IStream pStream = null;

                pStg.CreateStream(StreamName, (uint)
                   (STGM.DIRECT | STGM.CREATE |
                  STGM.READWRITE | STGM.SHARE_EXCLUSIVE),

                    0, 0, out pStream);

 

                if (pStream == null)

                    returnfalse ;

 

                byte[] byteVsize =

                    System.BitConverter.GetBytes
                                    (data.Length);              

                byte[] byteVData =

                    Encoding.Default.GetBytes(data);

                uint dummy;

 

    // convert string to byte and store it to the stream

                pStream.Write(byteVsize,

                    (uint)(sizeof(int)),

                    out dummy);

                pStream.Write(byteVData,

                    (uint)(byteVData.Length),

                    out dummy);              

 

                // Save the data          

                pStream.Commit((uint)
                         (MVOI.STGC.STGC_OVERWRITE |

                          MVOI.STGC.STGC_DEFAULT));

 

          //Don't forget to commit changes also in storage

                pStg.Commit((uint)(MVOI.STGC.STGC_DEFAULT |  
                         MVOI.STGC.STGC_OVERWRITE));

 

                // force document to be dirty thus

                // the change can be saved when document
               //is saved.

                pDoc.Dirty = true;               

                pDoc.Save();

 

                //Don't forget to release the object!!

                Marshal.ReleaseComObject(pStg);

 

                returntrue;

            }

            catch (Exception ex)

            {

                MessageBox.Show(ex.ToString());

                returnfalse;

            }

        }

 

        // read the storge and stream

        bool ReadPrivateStorageAndStream(Document pDoc,

            string StorageName,

            string StreamName,

              outstring  outDataStr)

        {

            outDataStr = "";

            try

            {              

                //get the storge. "false" means do not create
               //if it does not exist

                MVOI.IStorage pStg =

                    (MVOI.IStorage)pDoc.GetPrivateStorage
                         (StorageName, false);

                if (pStg == null)

                    returnfalse;

 

                // open stream to read

                MVOI.IStream pStream = null;

                pStg.OpenStream(StreamName,IntPtr.Zero,

                    (uint)(STGM.DIRECT| STGM.READWRITE |
                            STGM.SHARE_EXCLUSIVE),

                    0,  out pStream);

 

                if (pStream == null)

                    returnfalse;

 

                byte[] byteVsize = newbyte[16];

                uint intSize = sizeof(int);

 

                // read the stream

                uint dummy;

                pStream.Read(byteVsize,

                    (uint)intSize, out dummy);

                int lSize = System.BitConverter.ToInt16
                                     (byteVsize,0);

 

                byte[] outDataByte =

                    newbyte[8192];

                pStream.Read(outDataByte,

                    (uint)lSize, out dummy);

 

                // convert byte to string

                outDataStr =

                    Encoding.Default.GetString(outDataByte,
                                               0, lSize);

 

                //Don't forget to release the object!!

                Marshal.ReleaseComObject(pStg);

                returntrue;  

            }

            catch (Exception ex)

            {

            MessageBox.Show(ex.ToString());               

                returnfalse;

            }

 

        }

 

        // main function to test

        privatevoid test()

        {

            //get Inventor application

            string progId = "Inventor.Application";

            Inventor.Application m_inventorApp =

               (Inventor.Application)Marshal.GetActiveObject
                                               (progId );

 

            //get the current document.             

            Document pDoc = m_inventorApp.ActiveDocument;

 

            //create the storage and stream

            bool Result  = CreatePrivateStorageAndStream
                                (pDoc,

                                "MyPrvStorage1",

                                "MyStream1",

                                "Some private stored data");

 

            if (Result)

            {

                pDoc = m_inventorApp.ActiveDocument;

                string outPutStr = null;

                //read the storage and stream

                bool readResult = ReadPrivateStorageAndStream
                                (pDoc,

                                "MyPrvStorage1",

                                "MyStream1", out outPutStr);

 

                MessageBox.Show(outPutStr);

            }

        }

    

Last, I’d like to point out a tool Structured Storage Viewer which even enables you to read/write data without Inventor. It also proves that you can read/write this data programmatically without using any Inventor API because Inventor file is also a kind of Windows file:
 http://download.cnet.com/Structured-Storage-Viewer/3000-2248_4-75649632.html

Manipulate rows and columns of iPart - 2

By Xiaodong Liang

The last post introduces how to create and configure the iPart table. In this post, we take a look how to manipulate the existing iPart table. It is very straightforward. You just need to add/remove rows/columns in the Excel sheet.

Following test demo is based on the code in the last post . We delete the third column, add a row to the end of the iPart table and delete the second row.

 

Public Sub test() 
    'Create an iPart table (21 row, 6 columns) 
    CreateNewiPartTable  ' please refer to the last post 
    'Delete the third column 
    DeleteColumn 3 
    'Add a row to the end of the iPart table 
    AddRow 
    'Delete the second row 
    DeleteRow 2 
End Sub 

Private Sub DeleteColumn(indexOfColumn As Integer) 
    Dim oPartDoc As PartDocument 
    Set oPartDoc = ThisApplication.ActiveDocument 
    On Error Resume Next 
    Dim oFactory As iPartFactory 
    Set oFactory = oPartDoc.ComponentDefinition.iPartFactory 
    'Get the iPartTable 
    If Err > 0 Or oFactory Is Nothing Then 
        Exit Sub 
    End If 
    On Error GoTo 0 
    ' get the column by the index 
    Dim column As iPartTableColumn 
    Set column = oFactory.TableColumns.Item(indexOfColumn) 
    If Not column Is Nothing Then 
        Dim oWorkSheet As WorkSheet 
        Set oWorkSheet = oFactory.ExcelWorkSheet 
        Dim oCells As Range 
        Set oCells = oWorkSheet.Cells 
        Dim oCell As Range 
        Set oCell = oWorkSheet.Columns(indexOfColumn) 
        oCell.Delete 
        Dim oWB As WorkBook 
        Set oWB = oWorkSheet.Parent 
        oWB.Save 
        oWB.Close 
    End If 
    MsgBox "delete a column - done!" 
End Sub

Private Sub DeleteRow(indexOfRow As Integer) 
    Dim oPartDoc As PartDocument 
    Set oPartDoc = ThisApplication.ActiveDocument 
    On Error Resume Next 
    Dim oFactory As iPartFactory 
    Set oFactory = oPartDoc.ComponentDefinition.iPartFactory 
    'Get the iPartTable 
    If Err > 0 Or oFactory Is Nothing Then 
        Exit Sub 
    End If 
    On Error GoTo 0 
    Dim row As iPartTableRow 
    Set row = oFactory.TableRows.Item(indexOfRow) 
    If Not row Is Nothing Then 
        row.Delete 
    End If 
    MsgBox "delete a row - done!" 
End Sub 

Private Sub AddRow() 
    Dim oPartDoc As PartDocument 
    Set oPartDoc = ThisApplication.ActiveDocument 
    On Error Resume Next 
    Dim oFactory As iPartFactory 
    Set oFactory = oPartDoc.ComponentDefinition.iPartFactory 
    'Get the iPartTable 
    If Err > 0 Or oFactory Is Nothing Then 
     Exit Sub 
    End If 
    'Get the part number used in the iPart table 
    Dim row As iPartTableRow 
    Set row = oFactory.TableRows.Item(oFactory.TableRows.Count) 
    Dim sPartNumber As String 
    If Not row Is Nothing Then 
        sPartNumber = row.MemberName 
    End If 
    Dim pos As Integer 
    pos = InStrRev(sPartNumber, "-") 
    Dim str As String 
    str = Left(sPartNumber, pos) 
    Dim iNumber As Integer 
    iNumber = Right(sPartNumber, Len(sPartNumber) - pos) 
    'Assume the offset of the parameter's value (between two rows) is 0.5cm 
    Dim offset As Double 
    offset = 0.5 
    Dim oWorkSheet As WorkSheet 
    Set oWorkSheet = oFactory.ExcelWorkSheet 
    Dim oCells As Range 
    Set oCells = oWorkSheet.Cells 
    ' New row's value... 
    If (iNumber + 1) < 10 Then 
        sPartNumber = str + "0" + CStr(iNumber + 1) 
    Else 
        sPartNumber = str + CStr(iNumber + 1) 
    End If 
    Dim oCell As Range 
    Set oCell = oCells.Insert(, True) 
    oCells.Item(row.Index + 2, 1) = sPartNumber 
    oCells.Item(row.Index + 2, 2) = sPartNumber 
    Dim oUM As UnitsOfMeasure 
    Set oUM = oPartDoc.UnitsOfMeasure 
    Dim i As Integer 
    Dim oParameter As Parameter 
    For i = 3 To oCells.Columns.Count 
        Set oParameter = oPartDoc.ComponentDefinition.Parameters.ModelParameters.Item(oCells.Item(1, i).Value) 
        If oParameter.Name <> oPartDoc.ComponentDefinition.Parameters.ModelParameters.Item(4).Name Then 
            oCells.Item(row.Index + 2, i) = oUM.GetStringFromValue(oParameter.Value + offset * (row.Index), oParameter.Units) 
        Else 
            oCells.Item(row.Index + 2, i) = oPartDoc.ComponentDefinition.Parameters.ModelParameters.Item(4).Expression 
        End If 
    Next 
    Set oUM = Nothing 
    Dim oWB As WorkBook 
    Set oWB = oWorkSheet.Parent 
    oWB.Save 
    oWB.Close 
    MsgBox "Add a row - done!" 
End Sub

Save extra data in Inventor file – 2

By Xiaodong Liang

The second mechanism is attributes. Attributes allow you to attach
information to a specific object. Attributes can be associated with the Document object so you can use this to store general information associated with the document.

Attributes has been widely introduced in various articles. I’d recommend:

- API help reference >> [Attributes]

 

- Introduction to Attributes on Brian’s blog

http://modthemachine.typepad.com/my_weblog/2009/07/introduction-to-attributes.html

In short:

Creating AttributeSet and Attributes

- From AttributeSets Collection add a new AttributeSet :

Public Function Add(
             ByVal AttributeSetName As String,    
             Optional ByVal CopyWithOwner As Boolean = False )
              As AttributeSet

- From AttributeSet Collection add a new Attribute:

Public Function Add(
              ByVal AttributeName As String,
              ByVal ValueType As ValueTypeEnum,
              ByVal Value As Variant ) As Attribute

ValueTypeEnum: 
    kIntegerType
    kDoubleType
    kStringType
    kByteArrayType
    kBooleanType

Querying Attributes
AttributeManager supports different methods to query for attributes.
Can query based on attribute set name, attribute name, and/or attribute value.

   FindAttributes
   FindAttributeSets
   FindObjects

e.g.
Public Function FindObjects(
    Optional ByVal AttributeSetName As String = "*",    
    Optional ByVal AttributeName As String = "*",    
     Optional ByVal AttributeValue As Variant ) As ObjectCollection

 

Similar to the first post, In this post, we write a small demo to add a custom attribute set with some attributes. It also shows how to read the information.

VBA

Sub AddCustomAttribute()

    ' open a document invisible
    Dim oDoc As Document
     Set oDoc = ThisApplication.Documents.Open("c:\testpart.ipt", False)

    ' name of new attribute set
    Dim oNameOfNewPS As String
    oNameOfNewPS = "myNewSet"
    ' new attribute set
    Dim oNewPS As AttributeSet
    If oDoc.AttributeManager.FindAttributeSets(oNameOfNewPS).Count > 0 Then
       ' if the set exists aleady
       Set oNewPS = oDoc.AttributeSets(oNameOfNewPS)
       ' you can clean up the existing attributes
    Else
        ' add a new one
         Set oNewPS = oDoc.AttributeSets.Add(oNameOfNewPS)
     End If

    'the values of the attributes
    Dim oIntProV As Integer
    oIntProV = 100
    Dim oByteProV() As Byte
    oByteProV = StrConv("ABCDEFG", vbFromUnicode)
     Dim oDoubleProV As Double
    oDoubleProV = 3.1415926
    Dim oDateProV As String
    oDateProV = "2013-3-1 15:25"

    ' add these attributes with the meaningful name
    ' assume they do not exist in the attribute set
    Call oNewPS.Add("ModelCount", kIntegerType, oIntProV)
    Call oNewPS.Add("ModelByte", kByteArrayType, oByteProV)
    Call oNewPS.Add("ModelBasicLength", kDoubleType, oDoubleProV)
    Call oNewPS.Add("ModelUpdateDate", kStringType, oDateProV)
    oDoc.Save
    oDoc.Close
End Sub

Sub ReadCustomAttribute()

      ' open a document invisible
    Dim oDoc As Document
    Set oDoc = ThisApplication.Documents.Open("c:\testpart.ipt", False)
    ' name of new attribute set
    Dim oNameOfNewPS As String
    oNameOfNewPS = "myNewSet"
    ' new attribute set
    Dim oNewPS As AttributeSet
    If oDoc.AttributeManager.FindAttributeSets(oNameOfNewPS).Count > 0 Then
       ' if the set exists aleady
       Set oNewPS = oDoc.AttributeSets(oNameOfNewPS)
      ' you can clean up the existing attributes
    Else
        MsgBox "no attribute set named myNewSet"
        Exit Sub
    End If
    Dim oShowStr As String
    oShowStr = ""

    'iterate the attributes
    Dim oEachAtt As Attribute
    For Each oEachAtt In oNewPS
       oShowStr = oShowStr & " [Attribute Name]  " & oEachAtt.Name
       If oEachAtt.Name = "ModelByte" Then
        oShowStr = oShowStr & " [Attribute Value]  " & StrConv(oEachAtt.Value, vbUnicode) & vbCr
       Else
        oShowStr = oShowStr & " [Attribute Value]  " & oEachAtt.Value & vbCr
       End If
    Next
    MsgBox oShowStr
    oDoc.Close
End Sub

VB.NET

    Sub AddCustomAttribute()

 

        Dim m_inventorApp As Inventor.Application = Nothing

        m_inventorApp = System.Runtime.InteropServices.Marshal.GetActiveObject("Inventor.Application")

 

 

        ' open a document invisible

        Dim oDoc As Document

        oDoc = m_inventorApp.Documents.Open("c:\testpart.ipt", False)

 

 

        ' name of new attribute set

        Dim oNameOfNewPS As String

        oNameOfNewPS = "myNewSet"

 

        ' new attribute set

        Dim oNewPS As AttributeSet

        If oDoc.AttributeManager.FindAttributeSets(oNameOfNewPS).Count > 0 Then

            ' if the set exists aleady

            oNewPS = oDoc.AttributeSets(oNameOfNewPS)

            ' you can clean up the existing attributes

        Else

            ' add a new one

            oNewPS = oDoc.AttributeSets.Add(oNameOfNewPS)

        End If

 

 

        'the values of the attributes

        Dim oIntProV As Integer

        oIntProV = 100

        Dim oByteProV() As Byte

        oByteProV = System.Text.Encoding.Default.GetBytes("ABCDEFG")

        Dim oDoubleProV As Double

        oDoubleProV = 3.1415926

        Dim oDateProV As String

        oDateProV = "2013-3-1 15:25"

 

        ' add these attributes with the meaningful name

        ' assume they do not exist in the attribute set

        Call oNewPS.Add("ModelCount", ValueTypeEnum.kIntegerType, oIntProV)

        Call oNewPS.Add("ModelByte", ValueTypeEnum.kByteArrayType, oByteProV)

        Call oNewPS.Add("ModelBasicLength", ValueTypeEnum.kDoubleType, oDoubleProV)

        Call oNewPS.Add("ModelUpdateDate", ValueTypeEnum.kStringType, oDateProV)

        oDoc.Save()

        oDoc.Close()

    End Sub

 

    Sub ReadCustomAttribute()

 

        Dim m_inventorApp As Inventor.Application = Nothing

        m_inventorApp = System.Runtime.InteropServices.Marshal.GetActiveObject("Inventor.Application")

 

 

        ' open a document invisible

        Dim oDoc As Document

        oDoc = m_inventorApp.Documents.Open("c:\testpart.ipt", False)

 

        ' name of new attribute set

        Dim oNameOfNewPS As String

        oNameOfNewPS = "myNewSet"

 

        ' new attribute set

        Dim oNewPS As AttributeSet

        If oDoc.AttributeManager.FindAttributeSets(oNameOfNewPS).Count > 0 Then

            ' if the set exists aleady

            oNewPS = oDoc.AttributeSets(oNameOfNewPS)

            ' you can clean up the existing attributes

        Else

            MsgBox("no attribute set named myNewSet")

            Exit Sub

        End If

 

        Dim oShowStr As String

        oShowStr = ""

 

        'iterate the attributes

        Dim oEachAtt As Attribute

        For Each oEachAtt In oNewPS

            oShowStr = oShowStr & " [Attribute Name]  " & oEachAtt.Name

            If oEachAtt.Name = "ModelByte" Then

                oShowStr = oShowStr & " [Attribute Value]  " & System.Text.Encoding.Default.GetString(oEachAtt.Value) & vbCr

            Else

                oShowStr = oShowStr & " [Attribute Value]  " & oEachAtt.Value & vbCr

            End If

 

        Next

        MessageBox.Show(oShowStr)

        oDoc.Close()

    End Sub

Apprentice

    Sub AddCustomAttribute_Apprentice()

 

        Dim m_ApprenticeApp As Inventor.ApprenticeServerComponent =

             New Inventor.ApprenticeServerComponent()

 

        ' open a document invisble

        ' open a document

        Dim oDoc As ApprenticeServerDocument

        oDoc = m_ApprenticeApp.Open("c:\testpart.ipt")

 

 

        ' name of new attribute set

        Dim oNameOfNewPS As String

        oNameOfNewPS = "myNewSet"

 

        ' new attribute set

        Dim oNewPS As AttributeSet

        If oDoc.AttributeManager.FindAttributeSets(oNameOfNewPS).Count > 0 Then

            ' if the set exists aleady

            oNewPS = oDoc.AttributeSets(oNameOfNewPS)

            ' you can clean up the existing attributes

        Else

            ' add a new one

            oNewPS = oDoc.AttributeSets.Add(oNameOfNewPS)

        End If

 

 

        'the values of the attributes

        Dim oIntProV As Integer

        oIntProV = 100

        Dim oByteProV() As Byte

        oByteProV = System.Text.Encoding.Default.GetBytes("ABCDEFG")

        Dim oDoubleProV As Double

        oDoubleProV = 3.1415926

        Dim oDateProV As String

        oDateProV = "2013-3-1 15:25"

 

        ' add these attributes with the meaningful name

        ' assume they do not exist in the attribute set

        Call oNewPS.Add("ModelCount", ValueTypeEnum.kIntegerType, oIntProV)

        Call oNewPS.Add("ModelByte", ValueTypeEnum.kByteArrayType, oByteProV)

        Call oNewPS.Add("ModelBasicLength", ValueTypeEnum.kDoubleType, oDoubleProV)

        Call oNewPS.Add("ModelUpdateDate", ValueTypeEnum.kStringType, oDateProV)

 

        m_ApprenticeApp.FileSaveAs.AddFileToSave(oDoc, oDoc.FullDocumentName)

        m_ApprenticeApp.FileSaveAs.ExecuteSave()

    End Sub

 

    Sub ReadCustomAttribute_Apprentice()

 

        Dim m_ApprenticeApp As Inventor.ApprenticeServerComponent =

              New Inventor.ApprenticeServerComponent()

 

        ' open a document invisble

        ' open a document

        Dim oDoc As ApprenticeServerDocument

        oDoc = m_ApprenticeApp.Open("c:\testpart.ipt")

 

        ' name of new attribute set

        Dim oNameOfNewPS As String

        oNameOfNewPS = "myNewSet"

 

        ' new attribute set

        Dim oNewPS As AttributeSet

        If oDoc.AttributeManager.FindAttributeSets(oNameOfNewPS).Count > 0 Then

            ' if the set exists aleady

            oNewPS = oDoc.AttributeSets(oNameOfNewPS)

            ' you can clean up the existing attributes

        Else

            MsgBox("no attribute set named myNewSet")

            Exit Sub

        End If

 

        Dim oShowStr As String

        oShowStr = ""

 

        'iterate the attributes

        Dim oEachAtt As Attribute

        For Each oEachAtt In oNewPS

            oShowStr = oShowStr & " [Attribute Name]  " & oEachAtt.Name

            If oEachAtt.Name = "ModelByte" Then

                oShowStr = oShowStr & " [Attribute Value]  " & System.Text.Encoding.Default.GetString(oEachAtt.Value) & vbCr

            Else

                oShowStr = oShowStr & " [Attribute Value]  " & oEachAtt.Value & vbCr

            End If

 

        Next

        MessageBox.Show(oShowStr)

        oDoc.Close()

    End Sub