Manufacturing DevBlog

Access to the Bill Of Materials from a Different Level Of Details than Master

By Barbara Han

Though you have access to the BOM object through AssemblyComponentDefinition.BOM even in case of a document which is using a LOD (Level Of Detail) other than the Master, this only provides access to the "Model Data" view ("Unnamed"/kModelDataBOMViewType).

The "Structured" and "Parts Only" BOMView objects can only be accessed from a Master LOD document. So if the currently open assembly document is using a LOD other than the Master, then you can open its Master LOD version in the background and access those BOM views from there.

The below code sample shows how to do it:

VB.NET

Public Sub BOMQuery()

  Dim m_inventorApp As Inventor.Application = Nothing

  ' Try to get an active instance of Inventor

  Try

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

  Catch ex As Exception

  End Try

  ' If not active, create a new Inventor session

  If m_inventorApp Is Nothing Then

    Dim inventorAppType As Type = System.Type.GetTypeFromProgID("Inventor.Application")

    m_inventorApp = System.Activator.CreateInstance(inventorAppType)

  End If

  Dim oDoc As AssemblyDocument

  Dim oBOM As BOM

 

  ' Set a reference to the assembly document.

  ' This assumes an assembly document is active.

  oDoc = m_inventorApp.ActiveDocument

 

  'Gets back Master LOD

  Dim oAsmDocMasterLOD As AssemblyDocument

  oAsmDocMasterLOD = m_inventorApp.Documents.Open(oDoc.File.FullFileName, False)

  'Obtains BOM from Master LOD only

  oBOM = oAsmDocMasterLOD.ComponentDefinition.BOM

  'From here you can operate on the BOM object...

  'Following lines of code are examples only

  ' Set whether first level only or all levels

  oBOM.StructuredViewFirstLevelOnly = True

 

  ' Make sure that the structured view is enabled

  oBOM.StructuredViewEnabled = True

  MsgBox("BOM Views: " & oBOM.BOMViews.count)

End Sub

VBA

Public Sub BOMQuery()

Dim oDoc As AssemblyDocument
Dim oBOM As BOM

' Set a reference to the assembly document.
' This assumes an assembly document is active.
Set oDoc = ThisApplication.ActiveDocument

'Gets back Master LOD
Dim oAsmDocMasterLOD As AssemblyDocument
Set oAsmDocMasterLOD = ThisApplication.Documents.Open(oDoc.file.FullFileName, False)
'Obtains BOM from Master LOD only
Set oBOM = oAsmDocMasterLOD.ComponentDefinition.BOM

'From here you can operate on the BOM object...
'Following lines of code are examples only

' Set whether first level only or all levels
oBOM.StructuredViewFirstLevelOnly = True

' Make sure that the structured view is enabled
oBOM.StructuredViewEnabled = True

MsgBox "BOM Views: " & oBOM.BOMViews.count
End Sub

// Edited by Adam Nagy

Replace a Component in an Assembly and Maintain Constraints Using the API

By Barbara Han

To replace a component via the Inventor API, you can use the ComponentOccurrence.Replace method. This method takes two parameters:

1. The full file name of the file to be used to replace the existing occurrence.
2. A Boolean value that indicates whether the current occurrence should be replaced or all the instances of this occurrence.

When replacing occurrences, the behavior is the same as that of the Replace command from the Inventor UI. If the new file that you are replacing with is the same as the original one in geometry, the constraints will be maintained. If the geometry is different Inventor will not know how to keep the constraints and they will not be maintained. The following are the code sample from VB.NET and C#:

VB.NET

Private Sub ReplaceOccurrence()

 

  If m_inventorApplication.ActiveDocument.DocumentType <> DocumentTypeEnum.kAssemblyDocumentObject Then

    MsgBox("An assembly file must be open")

    Exit Sub

  End If

 

  'get the active assembly document

  Dim oAssemDoc As AssemblyDocument = m_inventorApplication.ActiveDocument

 

  'get the assembly component definition

  Dim oAssemDef As AssemblyComponentDefinition = oAssemDoc.ComponentDefinition

 

  'get the assembly occurrences

  Dim oCompOccs As ComponentOccurrences = oAssemDef.Occurrences

 

  If oCompOccs.Count = 0 Then

    MsgBox("Assembly does not contain any occurrence")

    Exit Sub

  End If

 

  'get the first occurrence

  Dim oCompOcc As ComponentOccurrence = oCompOccs(1)

 

  'replace the occurrence with another part/assembly (specify full file name)

  Call oCompOcc.Replace("C:\case\part1.ipt", False)

 

End Sub

C#

public void ReplaceOccurrence ()

{

    if (m_inventorApplication.ActiveDocument.DocumentType != DocumentTypeEnum.kAssemblyDocumentObject )

    {

        MessageBox.Show ("An assembly file must be open");

        return;

    }

 

    //get the active assembly document

    AssemblyDocument oAssemDoc = (AssemblyDocument)m_inventorApplication.ActiveDocument;

 

    //get the assembly component definition

    AssemblyComponentDefinition oAssemDef = oAssemDoc.ComponentDefinition;

 

    //get the assembly occurrences

    ComponentOccurrences oCompOccs = oAssemDef.Occurrences;

 

    if (oCompOccs.Count == 0)

    {

        MessageBox.Show("Assembly does not contain any occurrence");

        return;

    }

 

    //get the first occurrence

    ComponentOccurrence oCompOcc = oCompOccs[1];

 

    //replace the occurrence with another part/assembly (specify full file name)

    oCompOcc.Replace("C:\\case\\part1.ipt", false);

 

}

Note: In the case of the second parameter of Replace method being True (all instances of this occurrence are to be replaced), you can use the ReplaceReference method via apprentice API or Inventor API. This blog article illustrating this.

Replace the File Reference by Inventor API

By Barbara Han

Before Inventor 10 (including) the ReferenceFileDescriptor.PutCustomLogicalUsingFull was the method used to replace the file reference and this method was only allowed in Apprentice on non-migrating data sets.

But after Inventor 10, there is a new object called file object is introduced, where each File object will contain one or more documents. Now document is not the same as file anymore where the documents are still represented by the various document objects. So, hereafter instead of using ReferenceFileDescriptor.PutLogicalFilenameUsingFull we need to use FileDescriptor.ReplaceReference.

Significantly, FileDescriptor.ReplaceReference is available inside Inventor as well as in Apprentice.

Following is a part of VBA code which shows how to use the FileDescriptor.ReplaceReference with apprentice API:

Dim oApprentice As ApprenticeServerComponent
Set oApprentice = New ApprenticeServerComponent
Dim oADoc As ApprenticeServerDocument
Set oADoc = oApprentice.Open("C:\Assembly1.iam")
Dim oFD As FileDescriptor
Set oFD = oADoc.File.ReferencedFileDescriptors(1)
Call oFD.ReplaceReference("C:\Part2.ipt")
Call oApprentice.FileSaveAs.AddFileToSave(oADoc, oADoc.FullFileName)
Call oApprentice.FileSaveAs.ExecuteSave
 

And this is a part of VBA code that does the same with Inventor API:

Dim oDoc As Inventor.DrawingDocument
Set oDoc = ThisApplication.Documents.Open("C:\Assembly1.iam")

oDoc.File.ReferencedFileDescriptors(1).ReplaceReference("C:\Part2.ipt")

Note: For a file to be valid as a replacement it must have the same heritage as the file being replaced. You cannot replace a file with a brand new file. It has to be copied or modified from the already existing file - they must have shared the same ancestor in their past.

Get the Level Of Detail Representations Using Apprentice

By Barbara Han

Issue
I would like to know the Level Of Detail Representations before opening the assembly document. How could I do it using Apprentice?

Solution
You can use the RepresentationsManager from Apprentice, and all the read functions for objects under LevelOfDetailRepresentations should work fine. However, you can query all the available LevelOfDetailRepresentations using the FileManager as well, so you do not even need to open the document.
Below demonstrates two approaches:

1. Use FileManager:
Dim oASC As New ApprenticeServerComponent
 
' get the LODs without opening the document
Dim oDVRs As Variant
oDVRs = oASC.FileManager.GetLevelOfDetailRepresentations("C:\assy.iam")
 
Dim i As Integer
Debug.Print "Using FileManager"
For i = LBound(oDVRs) To UBound(oDVRs)
    Debug.Print oDVRs(i)
Next

2. Open file and use RepresentationsManager: 
' open the document
Dim oASD As ApprenticeServerDocument
Set oASD = oASC.Open("C:\assy.iam")
 

Dim oACD As AssemblyComponentDefinition
Set oACD = oASD.ComponentDefinition
 
Dim oRM As RepresentationsManager
Set oRM = oACD.RepresentationsManager
 
Dim oLOD As LevelOfDetailRepresentation
Debug.Print "Using RepresentationsManager"
For Each oLOD In oRM.LevelOfDetailRepresentations
    Debug.Print oLOD.Name
Next

Get All Referenced Files Using Inventor API

By Barbara Han

Issue
Is there a way to get all the referenced files using the Inventor API, instead of Apprentice Server API?

Solution
Yes, it is possible to get the all referenced files using inventor API. See the VBA code below which will give you all referenced files.

Sub reftest()
    Dim OApp As Inventor.Application
    Set OApp = GetObject(, "Inventor.Application")

    Dim oDoc As Document
    Set oDoc = OApp.ActiveDocument
    Dim oAllrefdocs As Documents
    Set oAllrefdocs = oDoc.ReferencedFiles

    Dim oSubDoc As Document
    Dim oSubDoc1 As Document
    Dim sMsg As String
    Dim iLeafNodes As Long
    Dim iSubAssemblies As Long

    For Each oSubDoc In oAllrefdocs
        If oSubDoc.ReferencedFileDescriptors.count = 0 Then
           Debug.Print oSubDoc.FullFileName
           iLeafNodes = iLeafNodes + 1
        Else
           Debug.Print oSubDoc.FullFileName
           iSubAssemblies = iSubAssemblies + 1
           Call processAllSubdoc(oSubDoc, _
                                 sMsg, _
                                 iLeafNodes, _
                                 iSubAssemblies)
        End If
    Next
End Sub

Sub processAllSubdoc(ByVal oSubDoc As Document, _
                             ByRef sMsg As String, _
                             ByRef iLeafNodes As Long, _
                             ByRef iSubAssemblies As Long)
    Dim oSubDoc1 As Document
    For Each oSubDoc1 In oSubDoc.ReferencedFiles
        ' Check if it's child occurrence (leaf node)
        If oSubDoc1.ReferencedFileDescriptors.count = 0 Then
            Debug.Print oSubDoc1.FullFileName
            iLeafNodes = iLeafNodes + 1
        Else
            sMsg = sMsg + oSubDoc1.Name + vbCr
            iSubAssemblies = iSubAssemblies + 1
            Call processAllSubdoc(oSubDoc1, _
                                  sMsg, _
                                  iLeafNodes, _
                                  iSubAssemblies)
        End If
    Next
End Sub

Prefer Rebuilds over Updates for Safety

By Barbara Han

Issue
Why should I prefer the Inventor API Document 'Rebuild()' method over the 'Update()' method? When should they yield the same result?

Solution
If you change a model via the Inventor API (e.g. change a constraint, or dimension or a parameter etc), then dependent entities need to be recomputed. This doesn't happen automatically (the benefit is that changes can be batched to re-compute operation to improve performance).
There are two methods that can be used to trigger a re-compute:

1. Update()
2. Rebuild()

Update() checks whether individual entities within the scope of the document require updating. Only those entities flagged as 'Dirty' are recomputed.
Rebuild() assumes that all entities are 'Dirty', and triggers a recompute on everything.
Update is quicker, because only those entities that require a re-compute receive one. However we are reliant on the logic inside Inventor being correct, and setting entities as 'Dirty' appropriately. This isn't always the case. Rebuild is slower, but it is safer. 
So as a general rule prefer Rebuild over Update for safety.
Use Update when there are performance implications to consider.

Replace a Part in Nested Sub-assembly by Inventor API

By Barbara Han

Assuming you have a assembly structure as shown below:

Main Assembly
         |
        +---Part1
         |
         ----sub-assembly
                    |
                    |
                   +---Part1

Now you want to replace part1.ipt in the sub-assembly by selecting it in the browser tree and then use the Replace command to replace it with Part2.ipt. 
How can we do the replacing through code? First, you have to traverse the assembly tree and check whether an occurrence is the selected one; then get the parent occurrence of the selected occurrence, that will be the sub-assembly, then use the index to get the occurrence from the definition of the parent occurrence; finally call the ComponentOccurrence.Replace() method.

The following sample code shown below demonstrates this. To test the code you need to create a similar assembly structure.

VBA code:

Public Sub ReplacePart()
       
    ' Get an occurrence from the select set.
    On Error Resume Next
    Dim oOccurrence As ComponentOccurrence
    Set oOccurrence = ThisApplication.ActiveDocument.SelectSet.Item(1)
    If Err Then
        MsgBox "An occurrence must be selected."
        Err.Clear
        On Error GoTo 0
        Exit Sub
    End If

    'get the parent of this occurrence
    Dim oParentOcc As ComponentOccurrence
    Set oParentOcc = oOccurrence.ParentOccurrence
   
    ' Now get the selected occurrence in scope of parent definition
    ' Make sure you got parent occurrence

    If (Not oParentOcc Is Nothing) Then
        Call getOccInScopeOfSubAsmDef(oParentOcc, oOccurrence)
        If (oOccurrence Is Nothing) Then
             Exit Sub
        End If
    End If
    ' Now replace will work as desired
   
    On Error Resume Next
    oOccurrence.Replace "d:\temp\replacetest\part2.ipt", False
    If Err Then
        Err.Clear
        On Error GoTo 0
        MsgBox "Failed to replace component"
    End If
End Sub

Private Sub getOccInScopeOfSubAsmDef(oParentOcc As ComponentOccurrence, ByRef oOccurrence As ComponentOccurrence)
    Dim indx As Integer
    indx = 1
    Dim bFound As Boolean
    bFound = False
    Dim oOcc As ComponentOccurrence
    For Each oOcc In oParentOcc.SubOccurrences
        If oOcc Is oOccurrence Then
            bFound = True
            Exit For
        End If
        indx = indx + 1
    Next
    If (bFound) Then
        Set oOccurrence = oParentOcc.Definition.Occurrences(indx)
    Else
        Set oOccurrence = Nothing
    End If
End Sub

VB.NET code:

public static void ReplacePart()
{
    try
    {
        Inventor.Application app = (Inventor.Application)System.Runtime.InteropServices.Marshal.GetActiveObject("Inventor.Application");

        // Get an occurrence from the select set.
        ComponentOccurrence oOccurrence = app.ActiveDocument.SelectSet[1] as ComponentOccurrence;

        //get the parent of this occurrence
        ComponentOccurrence oParentOcc = oOccurrence.ParentOccurrence;

        //Now get the selected occurrence in scope of parent definition
        // Make sure you got parent occurrence
        if (oParentOcc != null)
        {
            getOccInScopeOfSubAsmDef(oParentOcc, ref oOccurrence);

        }

        if (oOccurrence != null)
        {
            oOccurrence.Replace("c:\\temp\\replacetest\\part2.ipt", false);
        }
    }
    catch
    {
    }
}
public static void getOccInScopeOfSubAsmDef(ComponentOccurrence oParentOcc, ref ComponentOccurrence oOccurrence)
{
    int indx = 1;
    bool bFound = false;

    foreach(ComponentOccurrence oOcc in oParentOcc.SubOccurrences)
    {
        if(oOcc == oOccurrence)
        {
            bFound = true;
            break;
        }

        indx = indx + 1;
    }

    if (bFound)
    {
        oOccurrence = oParentOcc.Definition.Occurrences[indx];
    }
    else
    {
        oOccurrence = null;
    }
}

Use Inventor API to Get Drawing View Information Such as Scale , Referenced File etc

By Barbara Han

From a drawing document you can iterate through the Sheet collection object and from each Sheet object, retrieve all the drawing views, and from the drawing view you can extract further information. The sample code (VBA and C++) shown below prints information such as the scale of drawing view and file being referred by that view.

VBA code sample:

Sub getViewsInfo()
    Dim oDoc As Document
    Set oDoc = ThisApplication.ActiveDocument
   
    If oDoc.DocumentType = kDrawingDocumentObject Then
   
        Dim oDrgDoc As DrawingDocument
        Set oDrgDoc = oDoc
             
        Dim oSheets As Sheets
        Set oSheets = oDrgDoc.Sheets
        Dim oSheet As Sheet
       
        For Each oSheet In oSheets
            Dim oDrgViews As DrawingViews
            Set oDrgViews = oSheet.DrawingViews
            Dim oDrgView As DrawingView
            Dim msg As String
            Dim i As Integer
            i = 1
            For Each oDrgView In oDrgViews
                Dim scl As Double
                scl = oDrgView.Scale
                Dim oRefFileDesc As ReferencedFileDescriptor
                Set oRefFileDesc = oDrgView.ReferencedFile
               

                If (TypeOf oRefFileDesc.ReferencedDocument Is PartDocument) Then
                    Dim oPartDoc As PartDocument
                    Set oPartDoc = oRefFileDesc.ReferencedDocument
                ElseIf (TypeOf oRefFileDesc.ReferencedDocument Is AssemblyDocument) Then
                    Dim oAsmDoc As AssemblyDocument
                    Set oAsmDoc = oRefFileDesc.ReferencedDocument
                Else
                    Dim oPresDoc As PresentationDocument
                    Set oPresDoc = oRefFileDesc.ReferencedDocument
                End If
               
               
                msg = "View No: " & i & vbCr & _
                           "File Refered: " & oRefFileDesc.FullFileName & vbCr & _
                           "View Scale  : " & scl
                i = i + 1

               MsgBox msg
            Next
        Next
    End If
End Sub

C++ code sample:

HRESULT getViewsInfo()

{

 

  HRESULT hr = NOERROR;

 

  // Get active Inventor application

  TCHAR Str[_MAX_PATH];

 

  CLSID InvAppClsid;

  hr = CLSIDFromProgID (L"Inventor.Application", &InvAppClsid);

  if (FAILED(hr)) return hr;

 

  // Either create a new instance of the application or latch on to the currently active one.

  _tprintf_s (_T("Would you like to create a new Inventor application? (y/n) _: "));

  _tscanf_s (_T("%ls"), Str, _MAX_PATH);

 

  CComPtr<IUnknown> pInvAppUnk;

  if (toupper (Str[0]) == _T('Y'))

  {

    hr = CoCreateInstance (InvAppClsid, NULL, CLSCTX_LOCAL_SERVER, __uuidof(IUnknown), (void **) &pInvAppUnk);

    if (FAILED (hr))

      _tprintf_s (_T("*** Failed to create a new Inventor application ***\n"));

  }

  else

  {

    hr = ::GetActiveObject (InvAppClsid, NULL, &pInvAppUnk);

    if (FAILED (hr))

      _tprintf_s (_T("*** Could not get hold of an active Inventor application ***\n"));

  }

  if (FAILED(hr)) return hr;

 

  CComPtr<Application> m_pApplication;

  hr = pInvAppUnk->QueryInterface (__uuidof(Application), (void **) &m_pApplication);

  if (FAILED(hr)) return hr;

 

  CComPtr<Document> pDoc;

  hr=m_pApplication->get_ActiveDocument(&pDoc);

 

  if (pDoc != NULL && pDoc->DocumentType==kDrawingDocumentObject)

  { 

    CComQIPtr<DrawingDocument> pDrgDoc(pDoc);

 

    // Get sheets collection

    CComPtr<Sheets> pSheets;

    hr=pDrgDoc->get_Sheets(&pSheets);

    long nSheets=0;

    hr=pSheets->get_Count(&nSheets);

 

    // iterate through sheets

    for (long i =1 ; i <= nSheets ; i++)

    {

      CComPtr<Sheet> pSheet;

      hr=pSheets->get_Item(_variant_t(i),&pSheet);

 

      // Get drawing views collection

      CComPtr<DrawingViews> pDrawingViews;

      hr=pSheet->get_DrawingViews(&pDrawingViews);

 

      // iterate through drawing views

      long nViews=0;

      hr=pDrawingViews->get_Count(&nViews);

      for(long j =1 ; j <= nViews ; j++)

      {

        CComPtr<DrawingView> pDrawingView;

        hr=pDrawingViews->get_Item(j,&pDrawingView);

        double dScl = 0.0;

        hr=pDrawingView->get_Scale(&dScl);

 

        CComPtr<ReferencedFileDescriptor> pRefFileDesc;

        hr=pDrawingView->get_ReferencedFile(&pRefFileDesc);

 

        CComPtr<IUnknown> pUnk;

        hr=pRefFileDesc->get_ReferencedDocument(&pUnk); 

 

        // Now the referenced documnet can be ipt,iam or ipn

        // cast pUnk to document

        CComQIPtr<Document> pRefDoc(pUnk);

        if (pRefDoc->DocumentType==kPartDocumentObject)

          CComQIPtr<PartDocument> pPartDoc(pRefDoc);

        else if (pRefDoc->DocumentType==kAssemblyDocumentObject)

          CComQIPtr<AssemblyDocument> pAssmDoc(pRefDoc);

        else

          CComQIPtr<PresentationDocument> pPresDoc(pRefDoc);

 

        // Get the display name of reference document

        CComBSTR bstrFileName;

        hr=pRefFileDesc->get_FullFileName(&bstrFileName);

 

        _tprintf_s(_T("View No: %ld\nFile Refered: %s\nView Scale: %lf\n"), j,bstrFileName,dScl); 

      }

    }

  }

  return hr;

}

Update to Shortcut Key Customization Blog

By Barbara Han

Some times back, Gary posted a blog talking about “how to set the shortcut key to a customized command in Inventor”, however the code in that sample is quite out-of-date, so I want to give a update and also added one more point that you need to notice:

There are two types of shortcut key - Shortcut and Alias. Inventor API help document mentioned that the accelerator shortcut key can't be duplicate, but the alias shortcut key can. The alias shortcut key is interpreted as "Alt+<key>" (<key> is the letter showing in the Customize –> keyboard window), for instance, "I" alias shortcut key means that you can press Alt+I to bring out that command.

The following is a VBA code sample that assigns the alias shortcut key "I" to a custom command along with the code of deleting the command and custom ribbon. With VB.NET, the code is similar.

Below code is saved VBA Editor’s DocumentProject –>ThisDocument module:

Private WithEvents oBtnDef As ButtonDefinition

Sub AddBtnDefWithShortcut()

Dim oControlDefs As ControlDefinitions

Set oControlDefs = ThisApplication.CommandManager.ControlDefinitions

Dim ClientId As String
ClientId = "{3BB9D239-E672-4F2B-AA33-5B6A6EB74C54}"

'Create our own button command

Set oBtnDef = oControlDefs.AddButtonDefinition("MyControldefinition1", "Internal name for my controldef 1", kShapeEditCmdType, ClientId)

'Assign shortcut key to the button command

oBtnDef.OverrideShortcut = "I"

' Find the drawing ribbon.

Dim oRibbon As Ribbon

Set oRibbon = ThisApplication.UserInterfaceManager.Ribbons("Drawing")

Dim oRibbonTab As RibbonTab
Set oRibbonTab = oRibbon.RibbonTabs.Add("AdskRibbonTab", "AdskRibbonTab", ClientId)

' Add a control to the ribbon tab.
Dim oRibbonPanel As RibbonPanel
Set oRibbonPanel = oRibbonTab.RibbonPanels.Add("My Ribbon", "AdskRibbonPanel", ClientId)

Call oRibbonPanel.CommandControls.AddButton(oBtnDef)

End Sub

Private Sub oBtnDef_OnExecute(ByVal Context As NameValueMap)
    MsgBox ("command is running")
End Sub

Sub DeleteControlDef()

Dim oControlDefs As ControlDefinitions

Set oControlDefs = ThisApplication.CommandManager.ControlDefinitions

Dim oDef As ControlDefinition

Set oDef = oControlDefs.Item("Internal name for my controldef 1")

oDef.Delete

End Sub

Sub DeleteRibbon()
' Find the drawing ribbon.

Dim oRibbon As Ribbon

Set oRibbon = ThisApplication.UserInterfaceManager.Ribbons("Drawing")
Dim oRibbonTab As RibbonTab
Set oRibbonTab = oRibbon.RibbonTabs.Item("AdskRibbonTab")
Dim oRibbonPanel As RibbonPanel
Set oRibbonPanel = oRibbonTab.RibbonPanels.Item("AdskRibbonPanel")
oRibbonPanel.Delete
oRibbonTab.Delete
End Sub

Inventor and i-drop XML Package Format

By Barbara Han

I'm trying to publish some Inventor data in my website using i-drop. Here is an example which shows, at a bare minimum, what should be in there:

<?xml version = "1.0" encoding = "iso-8859-1"?>

<package>

    <proxy defaultsrc = "ebox.jpg">

        <caption>My Template of idrop Parts</caption>

    </proxy>

    <dataset defaultsrc = "ebox.ipt">

        <datasrc clipformat = "CF_IDROP.INV">

            <datafile src = "ebox.ipt"/>

            <Instructions>

                <Destination Pathtype = "parent" Pathname = ""/>

            </Instructions>

        </datasrc>

    </dataset>

</package>

The ebox.ipt file is a sample part file that comes from Inventor samples. Note that you'll need to specify the destination where a downloaded file should be stored relative to the currently active project:

<Instructions>
    <Destination Pathtype = "parent" Pathname = ""/>
</Instructions>

The Pathtype can be anyone of “parent workspace library workgroup temporary NoDownload”. The Inventor_iDrop_Schema_R2.0.xdr (XML format in nature) file has an explanation on these Pathtype. You can find this file in, for example C:\Users\Public\Documents\Autodesk\Inventor 2012\Web folder.

Next we need to create a html page to show the idrop with that part file. My sample html code is very simple:

<html>

<head>
<meta http-equiv="Content-Language" content="en-us">
<meta http-equiv="Content-Type" content="text/html; charset=windows-1252">
<title>Inventor iDrop WebTemplate</title>
</head>

<body>
  <p align="center">
    <object classid="clsid:21E0CB95-1198-4945-A3D2-4BF804295F78" codebase="http://www.autodesk.com/prods/idrop/download/idrop.cab">
      <param name="package" value="ebox.xml"/>
    </object>
  <BR>
  A copy of the file without modification&nbsp; is delivered to the location
  containing the parent assembly using the original filename.
</body>

</html>

With all the files (ebox.ipt, ebox.jpg) above mentioned in place, the idrop works.

Note: We presume that you have some embedding ActiveX control into HTML experience plus some JavaScript or VBScript experience. In addition, you should allow blocked the i-drop ActiveX control running on your web page.

The following is the running result: (the left is my web page, and the right is the assembly with the part from the left web page.)